Heidenhain MP620/CP640 (54843x-03 /68894x-03) smart.Turn/DIN CNC Control User Manual

User’s Manual
MANUALplus 620
CNC PILOT 640
smart.Turn and
DIN Programming
NC Software
548430-03
548431-03
688946-03
688947-03
HEIDENHAIN MANUALplus 620, CNC PILOT 620/640
1
English (en)
11/2014
smart.Turn and DIN PLUS
programming
This manual describes functions and features provided by lathe
controls as of the following NC software numbers.
Control
NC software number
MANUALplus 620 (HEROS 5)
548430-03
MANUALplus 620E (HEROS 5)
548431-03
CNC PILOT 640 (HEROS 5)
688946-03
CNC PILOT 640E (HEROS 5)
688947-03
The suffix E indicates the export version of the control. The export
version of the control has the following limitations:
 Simultaneous linear movement in up to 4 axes
HEROS 5 identifies the new operating system of HSCI-based controls.
Machine operation and cycle programming are described in the
MANUALplus 620 (ID 634864-xx) and CNC PILOT 640 (ID 730870-xx)
User's Manuals. Please contact HEIDENHAIN if you require a copy of
one of these manuals.
The machine manufacturer adapts the features offered by the control
to the capabilities of the specific machine tool by setting machine
parameters. Therefore, some of the functions described in this manual
may not be among the features provided by the Steuerung on your
machine tool.
Some of the Steuerung functions that are not available on every
machine are:
 Positioning of spindle (M19) and driven tool
 Operations with the C or Y axis
Please contact your machine manufacturer for detailed information on
the features that are supported by your machine tool.
Many machine manufacturers and HEIDENHAIN offer programming
courses. We recommend these courses as an effective way of
improving your programming skill and sharing information and ideas
with other Steuerung users.
HEIDENHAIN also offers the DataPilot programming station for PCs,
which is designed for use with the respective control. The DataPilot
is excellently suited for both shop-floor programming as well as offlocation program creation and production planning. It is also ideal for
training purposes. The DataPilot can be run on PCs with WINDOWS
operating systems.
Control
Programming station NC software
MANUALplus 620 DataPilot MP620
634132-07
CNC PILOT 640
729666-03
DataPilot CP640
Intended place of operation
The MANUALplus 620, CNC PILOT 640 complies with the limits for a
Class A device in accordance with the specifications in EN 55022, and
is intended for use primarily in industrially-zoned areas.
Legal information
This product uses open source software. Further information is
available on the control under



Organization mode of operation
Second soft-key row
LICENSE INFO SOFT KEY
HEIDENHAIN MANUALplus 620, CNC PILOT 640
3
New functions of software 54843x-01 and
68894x-01
 On machines with a B axis it is now also possible to drill, bore, and
mill in oblique planes. In addition to this, the B axis enables you to
use tools even more flexibly during turning (see „Tilted working
plane” on page 584).
 The control now provides numerous touch probe cycles for various
applications (see „General information on touch probe cycles
(software option)” on page 454):
 Calibrating a touch trigger probe
 Measuring circles, circle segments, angle and position of the C
axis
 Misalignment compensation
 Single-point and double-point measurement
 Finding a hole or stud
 Zero point setting in the Z or C axis
 Automatic tool measurement
 The new TURN PLUS function automatically generates NC
programs for turning and milling operations based on a fixed
machining sequence (see „TURN PLUS mode of operation” on
page 552).
 G940 now provides a way to calculate the tool lengths in the basic
(definition) position of the B axis (see „Calculate variables
automatically G940” on page 385)
 For machining operations that require rechucking, you can define a
separation point on the contour description with G44 (see
„Separation point G44” on page 222).
 G927 enables you to convert tool lengths to the reference position
of the tool (B axis = 0) (see „Convert lengths G927” on page 385).
 Recesses that were defined with G22 can now be machined with
the new Cycle 870 ICP Recessing (see „"ICP recessing" unit” on
page 79).
4
New functions of software 68894x-02 and
54843x-02
 The miscellaneous function "Shift zero point" was introduced in ICP
(see User's Manual)
 In ICP contours, you can now calculate fit sizes and internal threads
using an input form (see User's Manual)
 The miscellaneous functions "Duplicate in linear/circular series, and
by mirroring" were introduced in ICP (see User's Manual)
 The system time can now be set using an input form (see User's
Manual)
 The parameters K, SD and U have been added to parting cycle G859
(see User's Manual)
 The angle of approach and departure can now be defined for ICP
recess turning (see User's Manual)
 With TURN PLUS you can now also create programs for machining
on the opposing spindle and for multipoint tools (see „Full-surface
machining with TURN PLUS” on page 578)
 It is now also possible to select a milling contour in G797 "Area
milling" (see „Area milling, face G797” on page 355)
 The parameter Y was added to G720 (see „Spindle synchronization
G720” on page 392)
 The parameters O and U were added to G860 (see „Recessing
G860” on page 283)
HEIDENHAIN MANUALplus 620, CNC PILOT 640
5
New functions of software 68894x-03 and
54843x-03
 The parameter WE was added to G32 (see „Single thread cycle
G32” on page 307)
 The parameters U, V and W were added to G51, G56 and G59 (see
„Zero point shifts” on page 259)
 Parameters ensuring maximum compatibility with the ICP contour
description were added to G0, G1, G12/G13, G101, G102/G103,
G110, G111, G112/G113, G170, G171, G172/G173, G180, G181 and
G182/G183 (see „Basic contour elements” on page 201) (see
„Front and rear face contours” on page 230) (see „Lateral surface
contours” on page 239) (see „Contours in the XY plane” on page
504) (see „Contours in the YZ plane” on page 513)
 The parameter C was added to G808 (see „Hobbing G808” on page
543)
 The parameter U was added to G810 and G820 (see „Contourbased turning cycles” on page 270)
 The parameter D was added to G4 and G860 (see „Recessing
G860” on page 283) (see „Period of dwell G4” on page 381)
 The parameter B was added to G890 (see „Finish contour G890” on
page 290)
 The parameter RB was added to the units G840 "Contour milling,
figures" and G84X "Pocket milling, figures" (see „The Global form”
on page 64) (see „"Contour milling, figures, face" unit” on page 139)
(see „"Pocket milling, figures, face" unit” on page 142) (see
„"Contour milling, figures, lateral surface" unit” on page 151) (see
„"Pocket milling, figures, lateral surface" unit” on page 154)
 The parameters SP and SI were added to all tapping units (see
„Units—Centric drilling” on page 80) (see „Units—Drilling in C axis”
on page 84) (see „"ICP tapping, Y axis" unit” on page 169)
 G48 was introduced to allow limiting the rapid traverse rate for
rotary and linear axes (see „Reduce rapid traverse G48” on page
253)
 G53, G54 and G55 were introduced for zero point shifts using offset
values (see „Zero point offsets—Shift G53/G54/G55” on page 261)
 The functions for superimposing axis movements G725 "Eccentric
turning", G726 "Transition to eccentric" and G727 "Eccentric X" were
introduced (see „Eccentric turning G725” on page 399) (see
„Transition to eccentric G726” on page 401) (see „Eccentric X
G727” on page 403)
 The load monitoring functions G995 "Monitoring zone definition" and
G996 "Type of load monitoring" were introduced (see „Monitoring
zone G995” on page 388) (see „Load monitoring G996” on page
389)
 The AWG submode now also supports tools with quick-change
holders (see „Tool selection, turret assignment” on page 566)
 A tree view is available in the smart.Turn operating mode (see
„Editing with active tree view” on page 40)
 Skip levels can be defined in the smart.Turn operating mode (see
„Skip level” on page 426)
6
 A function was introduced to query information on the tool status
(see „Reading diagnostic bits” on page 413)
 In the Teach-In submode, the parameter RB was added to the cycles
"Figure, axial", "Figure, radial", "ICP contour, axial" and "ICP contour,
radial" (see User's Manual)
 In the Teach-In submode, the parameters SP and SI were added to
all tapping cycles (see User's Manual)
 The Simulation submode provides an enhanced 3-D view (see
User's Manual)
 Tool control graphics were introduced in the Tool Editor mode of
operation (see User's Manual)
 An ID number can be entered directly in the turret list (see User's
Manual)
 The tool list provides additional filter options (see User's Manual)
 The Transfer submode provides enhanced tool backup functionality
(see User's Manual)
 The Transfer submode provides enhanced tool import functionality
(see User's Manual)
 The Set Axis Values menu item now also enables you to define
offset values for shifts using G53, G54 and G55 (see User's Manual)
 Load monitoring was introduced in the Program Run submode (see
User's Manual)
 The definition of skip levels was introduced in the Program Run
submode (see User's Manual)
 A function was introduced to query information on the tool status
(see User's Manual)
 A user parameter was introduced to enable you to activate and
deactivate the software limit switches for the Simulation submode
(see User's Manual)
 A user parameter was introduced to enable you to suppress the
error message for the software limit switches (see User's Manual)
 A user parameter was introduced to enable you to use NC Start for
executing a tool change programmed in the T,S,F dialog (see User's
Manual)
 A user parameter was introduced to divide the T,S,F dialog into
separate dialogs (see User's Manual)
 A user parameter was introduced to enable you to prevent the zero
point shift G59 that is automatically output in TURN PLUS (see
User's Manual)
HEIDENHAIN MANUALplus 620, CNC PILOT 640
7
8
About this manual
About this manual
The symbols used in this manual are described below.
This symbol indicates that important information about the
function described must be considered.
This symbol indicates that there is one or more of the
following risks when using the described function:
 Danger to workpiece
 Danger to fixtures
 Danger to tool
 Danger to machine
 Danger to operator
This symbol indicates that the described function must be
adapted by the machine tool builder. The function
described may therefore vary depending on the machine.
This symbol indicates that you can find detailed
information about a function in another manual.
Would you like any changes, or have you found
any errors?
We are continuously striving to improve our documentation for you.
Please help us by sending your requests to the following e-mail
address: [email protected].
HEIDENHAIN MANUALplus 620, CNC PILOT 640
9
10
About this manual
Contents
„NC programming”
„smart.Turn units”
„smart.Turn units for the Y axis”
„DIN Programming”
„Touch probe cycles”
„DIN programming for the Y axis”
„TURN PLUS”
„B axis”
„Overview of units”
„Overview of G codes”
1
2
3
4
5
6
7
8
9
10
1 NC programming ..... 31
1.1 smart.Turn and DIN (ISO) programming ..... 32
Contour follow-up ..... 32
Structured NC program ..... 33
Linear and rotary axes ..... 34
Units of measure ..... 34
Elements of an NC program ..... 35
1.2 The smart.Turn editor ..... 36
Menu structure ..... 36
Parallel editing ..... 37
Screen layout ..... 37
Selecting the editor functions ..... 38
Editing with active tree view ..... 38
Shared menu items ..... 39
1.3 Program section code ..... 45
HEADER section ..... 46
CLAMPS section ..... 47
TURRET section ..... 48
BLANK section ..... 48
AUXIL_BLANK section ..... 48
FINISHED section ..... 48
AUXIL_CONTOUR section ..... 48
FACE_C, REAR_C sections ..... 49
LATERAL_C section ..... 49
FACE_Y, REAR_Y sections ..... 49
LATERAL_Y section ..... 50
MACHINING section ..... 51
END code ..... 51
SUBPROGRAM section ..... 51
RETURN code ..... 51
CONST code ..... 52
VAR code ..... 52
1.4 Tool programming ..... 53
Setting up a tool list ..... 53
Editing tool entries ..... 54
Multipoint tools ..... 54
Replacement tools ..... 55
HEIDENHAIN MANUALplus 620, CNC PILOT 640
13
2 smart.Turn units ..... 57
2.1 smart.Turn units ..... 58
"Units" menu ..... 58
The smart.Turn unit ..... 58
2.2 Units—Roughing ..... 65
"Longitudinal roughing in ICP" unit ..... 65
"Transverse roughing in ICP" unit ..... 66
"Contour-parallel roughing in ICP" unit ..... 67
"Bidirectional roughing in ICP" unit ..... 68
"Longitudinal roughing with direct contour input" unit ..... 69
"Transverse roughing with direct contour input" unit ..... 70
2.3 Units—Recessing ..... 71
"ICP contour recessing" unit ..... 71
"ICP recess turning" unit ..... 72
"Contour recessing with direct contour input" unit ..... 73
"Recess turning with direct contour input" unit ..... 74
"Parting" unit ..... 75
"Undercutting (H, K, U)" unit ..... 76
"ICP recessing" unit ..... 77
2.4 Units—Centric drilling ..... 78
"Centric drilling" unit ..... 78
"Centric tapping" unit ..... 80
"Boring, centric countersinking" unit ..... 81
2.5 Units—Drilling in C axis ..... 82
"Single hole, face" unit ..... 82
"Linear pattern drilling, face" unit ..... 84
"Circular pattern drilling, face" unit ..... 86
"Tapping, face" unit ..... 88
"Linear tapping pattern, face" unit ..... 89
"Circular tapping pattern, face" unit ..... 90
"Single hole, lateral surface" unit ..... 91
"Linear pattern drilling, lateral surface" unit ..... 93
"Circular pattern drilling, lateral surface" unit ..... 95
"Tap hole, lateral surface" unit ..... 97
"Linear tapping pattern, lateral surface" unit ..... 98
"Circular tapping pattern, lateral surface" unit ..... 99
"ICP drilling, C axis" unit ..... 100
"ICP tapping, C axis" unit ..... 102
"ICP boring/countersinking, C axis" unit ..... 103
14
2.6 Units—Predrilling in C axis ..... 104
"Predrill, contour mill, figures on face" unit ..... 104
"Predrill, contour mill, ICP on face" unit ..... 106
"Predrill, pocket mill, figures on face" unit ..... 107
"Predrill, pocket mill, ICP on face" unit ..... 109
"Predrill, contour mill, figures on lateral surface" unit ..... 110
"Predrill, contour mill, ICP on lateral surface" unit ..... 112
"Predrill, pocket mill, figures on lateral surface" unit ..... 113
"Predrill, pocket mill, ICP on lateral surface" unit ..... 115
2.7 Units—Finishing ..... 116
"ICP contour finishing" unit ..... 116
"Longitudinal finishing with direct contour input" unit ..... 118
"Transverse finishing with direct contour input" unit ..... 119
"Relief turns (undercut) type E, F, DIN76" unit ..... 120
"Measuring cut" unit ..... 122
2.8 Units—Threads ..... 123
Overview of thread units ..... 123
Handwheel superimposition ..... 123
Parameter V: Type of infeed ..... 124
"Thread, direct" unit ..... 125
"ICP thread" unit ..... 126
"API thread" unit ..... 128
"Tapered thread" unit ..... 129
2.9 Units—Milling, face ..... 131
"Slot, face" unit ..... 131
"Linear slot pattern, face" unit ..... 132
"Circular slot pattern, face" unit ..... 133
"Face milling" unit ..... 134
"Face milling ICP" unit ..... 135
"Thread milling" unit ..... 136
"Contour milling, figures, face" unit ..... 137
"ICP contour milling, face" unit ..... 139
"Pocket milling, figures, face" unit ..... 140
"ICP pocket milling, face" unit ..... 142
"Engraving, face" unit ..... 143
"Deburring, face" unit ..... 144
HEIDENHAIN MANUALplus 620, CNC PILOT 640
15
2.10 Units—Milling, lateral surface ..... 145
"Slot, lateral surface" unit ..... 145
"Linear slot pattern, lateral surface" unit ..... 146
"Circular slot pattern, lateral surface" unit ..... 147
"Helical slot milling" unit ..... 148
"Contour milling, figures, lateral surface" unit ..... 149
"ICP contour milling, lateral surface" unit ..... 151
"Pocket milling, figures, lateral surface" unit ..... 152
"ICP pocket milling, lateral surface" unit ..... 154
"Engraving, lateral surface" unit ..... 155
"Deburring, lateral surface" unit ..... 156
2.11 Units—Special operations ..... 157
"Program beginning (START)" unit ..... 157
"C axis ON" unit ..... 159
"C axis OFF" unit ..... 159
"Subprogram call" unit ..... 160
"Program section repeat" unit ..... 161
"Program end" unit ..... 162
"Tilt plane" unit ..... 163
16
3 smart.Turn units for the Y axis ..... 165
3.1 Units—Drilling in the Y axis ..... 166
"ICP drilling, Y axis" unit ..... 166
"ICP tapping, Y axis" unit ..... 167
"ICP boring/countersinking, Y axis" unit ..... 168
3.2 Units—Predrilling in Y axis ..... 169
"Predrill, contour mill, ICP in XY plane" unit ..... 169
"Predrill, pocket mill, ICP in XY plane" unit ..... 170
"Predrill, contour mill, ICP in YZ plane" unit ..... 171
"Predrill, pocket mill, ICP in YZ plane" unit ..... 172
3.3 Units—Milling in Y axis ..... 173
"ICP contour milling in XY plane" unit ..... 173
"ICP pocket milling in XY plane" unit ..... 174
"Single-surface milling, XY plane" unit ..... 175
"Centric polygon milling, XY plane" unit ..... 176
"Engraving in XY plane" unit ..... 177
"Deburring in XY plane" unit ..... 178
"Thread milling in XY plane" unit ..... 179
"ICP contour milling in YZ plane" unit ..... 180
"ICP pocket milling in YZ plane" unit ..... 181
"Single-surface milling, YZ plane" unit ..... 182
"Centric polygon milling, YZ plane" unit ..... 183
"Engraving in YZ plane" unit ..... 184
"Deburring in YZ plane" unit ..... 185
"Thread milling in YZ plane" unit ..... 186
HEIDENHAIN MANUALplus 620, CNC PILOT 640
17
4 DIN Programming ..... 187
4.1 Programming in DIN/ISO mode ..... 188
Geometry and machining commands ..... 188
Contour programming ..... 189
NC blocks of the DIN program ..... 190
Creating, editing and deleting NC blocks ..... 191
Address parameters ..... 192
Fixed cycles ..... 193
Subprograms, expert programs ..... 194
NC program conversion ..... 194
DIN/ISO programs of predecessor controls ..... 195
"Geometry" pull-down menus ..... 197
"Machining" pull-down menus ..... 197
4.2 Definition of workpiece blank ..... 198
Chuck part bar/tube G20-Geo ..... 198
Cast part G21-Geo ..... 198
4.3 Basic contour elements ..... 199
Starting point of turning contour G0-Geo ..... 199
Machining attributes for form elements ..... 199
Line segment in a contour G1-Geo ..... 200
Circular arc of turning contour G2/G3-Geo ..... 202
Circular arc of turning contour G12/G13-Geo ..... 203
4.4 Contour form elements ..... 205
Recess (standard) G22-Geo ..... 205
Recess (general) G23-Geo ..... 207
Thread with undercut G24-Geo ..... 209
Undercut contour G25-Geo ..... 210
Thread (standard) G34-Geo ..... 214
Thread (general) G37-Geo ..... 215
Bore hole (centric) G49-Geo ..... 217
4.5 Attributes for contour description ..... 218
Feed rate reduction G38-Geo ..... 218
Attributes for superimposed elements G39-Geo ..... 219
Separation point G44 ..... 220
Oversize G52-Geo ..... 220
Feed per revolution G95-Geo ..... 221
Additive compensation G149-Geo ..... 221
4.6 C-axis contours—Fundamentals ..... 222
Milling contour position ..... 222
Circular pattern with circular slots ..... 225
18
4.7 Front and rear face contours ..... 228
Starting point of front/rear face contour G100-Geo ..... 228
Line segment in front/rear face contour G101-Geo ..... 229
Circular arc in front/rear face contour G102/G103-Geo ..... 230
Bore hole on front/rear face G300-Geo ..... 231
Linear slot on front/rear face G301-Geo ..... 232
Circular slot on front/rear face G302/G303-Geo ..... 232
Full circle on front/rear face G304-Geo ..... 233
Rectangle on front/rear face G305-Geo ..... 233
Eccentric polygon on front/rear face G307-Geo ..... 234
Linear pattern on front/rear face G401-Geo ..... 235
Circular pattern on front/rear face G402-Geo ..... 236
4.8 Lateral surface contours ..... 237
Starting point of lateral surface contour G110-Geo ..... 237
Line segment in a lateral surface contour G111-Geo ..... 238
Circular arc in lateral surface contour G112/G113-Geo ..... 239
Hole on lateral surface G310-Geo ..... 240
Linear slot on lateral surface G311-Geo ..... 241
Circular slot on lateral surface G312/G313-Geo ..... 241
Full circle on lateral surface G314-Geo ..... 242
Rectangle on lateral surface G315-Geo ..... 242
Eccentric polygon on lateral surface G317-Geo ..... 243
Linear pattern on lateral surface G411-Geo ..... 244
Circular pattern on lateral surface G412-Geo ..... 245
4.9 Tool positioning ..... 246
Rapid traverse G0 ..... 246
Rapid traverse to machine coordinates G701 ..... 246
Approach tool change point G14 ..... 247
Definition of tool-change point G140 ..... 247
4.10 Linear and circular movements ..... 248
Linear movement G1 ..... 248
Circular path G2/G3 ..... 249
Circular path G12/G13 ..... 250
4.11 Feed rate, shaft speed ..... 251
Speed limitation G26 ..... 251
Reduce rapid traverse G48 ..... 251
Interrupted feed G64 ..... 252
Feed per tooth Gx93 ..... 252
Constant feed rate G94 (feed per minute) ..... 253
Feed per revolution Gx95 ..... 253
Constant surface speed Gx96 ..... 254
Speed Gx97 ..... 254
4.12 Tool-tip and cutter radius compensation ..... 255
G40: Switch off TRC/MCRC ..... 255
G41/G42: Switch on TRC/MCRC ..... 256
HEIDENHAIN MANUALplus 620, CNC PILOT 640
19
4.13 Zero point shifts ..... 257
Zero point shift G51 ..... 258
Zero point offsets—Shift G53/G54/G55 ..... 259
Additive zero point shift G56 ..... 259
Absolute zero point shift G59 ..... 260
4.14 Oversizes ..... 261
Switch off oversize G50 ..... 261
Axis-parallel oversize G57 ..... 261
Contour-parallel oversize (equidistant) G58 ..... 262
4.15 Safety clearances ..... 263
Safety clearance G47 ..... 263
Safety clearance G147 ..... 263
4.16 Tools, compensations ..... 264
Tool call T ..... 264
Correction of cut (switching the tool edge compensation) G148 ..... 265
Additive compensation G149 ..... 266
Compensation of right-hand tool tip G150
Compensation of left-hand tool tip G151 ..... 267
4.17 Contour-based turning cycles ..... 268
Working with contour-based cycles ..... 268
Longitudinal roughing G810 ..... 270
Face roughing G820 ..... 273
Contour-parallel roughing G830 ..... 276
Contour cycle, bidirectional (contour-parallel with neutral tool) G835 ..... 279
Recessing G860 ..... 281
Repeat recessing cycle G740/G741 ..... 283
Recess turning cycle G869 ..... 284
Recessing cycle G870 ..... 287
Finish contour G890 ..... 288
Measuring cut G809 ..... 291
4.18 Contour definitions in the machining section ..... 292
Cycle end / Simple contour G80 ..... 292
Linear slot on front/rear face G301 ..... 293
Circular slot on front/rear face G302/G303 ..... 293
Full circle on front/rear face G304 ..... 294
Rectangle on front/rear face G305 ..... 294
Eccentric polygon on front/rear face G307 ..... 295
Linear slot on lateral surface G311 ..... 295
Circular slot on lateral surface G312/G313 ..... 296
Full circle on lateral surface G314 ..... 296
Rectangle, lateral surface G315 ..... 297
Eccentric polygon, lateral surface G317 ..... 297
20
4.19 Thread cycles ..... 298
Overview of threading cycles ..... 298
Handwheel superimposition ..... 298
Parameter V: Type of infeed ..... 299
Thread cycle G31 ..... 301
Single thread cycle G32 ..... 305
Thread single path G33 ..... 307
Metric ISO thread G35 ..... 309
Tapered API thread G352 ..... 310
Metric ISO thread G38 ..... 312
4.20 Parting cycle ..... 313
Cut-off cycle G859 ..... 313
4.21 Undercut cycles ..... 314
Undercut cycle G85 ..... 314
Undercut according to DIN 509 E with cylinder machining G851 ..... 316
Undercut according to DIN 509 F with cylinder machining G852 ..... 317
Undercut according to DIN 76 with cylinder machining G853 ..... 318
Undercut type U G856 ..... 319
Undercut type H G857 ..... 320
Undercut type K G858 ..... 321
4.22 Drilling cycles ..... 322
Overview of drilling and boring cycles and contour reference ..... 322
Drilling cycle G71 ..... 323
Boring, countersinking G72 ..... 325
Tapping G73 ..... 326
Tapping G36—Single path ..... 328
Deep-hole drilling G74 ..... 329
Linear pattern, face G743 ..... 332
Circular pattern, face G745 ..... 333
Linear pattern, lateral surface G744 ..... 334
Circular pattern, lateral surface G746 ..... 335
Thread milling, axial G799 ..... 336
4.23 C-axis commands ..... 337
Reference diameter G120 ..... 337
Zero point shift, C axis G152 ..... 337
Standardize C axis G153 ..... 338
4.24 Front/rear-face machining ..... 339
Rapid traverse on front/rear face G100 ..... 339
Line segment on front/rear face G101 ..... 340
Circular arc on front/rear face G102/G103 ..... 341
4.25 Lateral surface machining ..... 343
Rapid traverse, lateral surface G110 ..... 343
Line segment on lateral surface G111 ..... 344
Circular arc on lateral surface G112/G113 ..... 345
HEIDENHAIN MANUALplus 620, CNC PILOT 640
21
4.26 Milling cycles ..... 346
Overview of milling cycles ..... 346
Linear slot on face G791 ..... 347
Linear slot on lateral surface G792 ..... 348
Contour and figure milling cycle, face G793 ..... 349
Contour and figure milling cycle, lateral surface G794 ..... 351
Area milling, face G797 ..... 353
Helical-slot milling G798 ..... 355
Contour milling G840 ..... 356
Pocket milling, roughing G845 ..... 366
Pocket milling, finishing G846 ..... 372
4.27 Engraving cycles ..... 374
Character set ..... 374
Engraving on front face G801 ..... 376
Engraving on lateral surface G802 ..... 377
4.28 Contour follow-up ..... 378
Saving/loading contour follow-up G702 ..... 378
Contour follow-up on/off G703 ..... 378
22
4.29 Other G codes ..... 379
Chucking equipment in simulation G65 ..... 379
Workpiece blank contour G67 (for graphics) ..... 379
Period of dwell G4 ..... 379
Precision stop G7 ..... 379
Precision stop off G8 ..... 380
Precision stop G9 ..... 380
Switch off protection zone G60 ..... 380
Actual values in variables G901 ..... 380
Zero-point shift in variables G902 ..... 380
Lag error in variables G903 ..... 380
Read interpolation information G904 ..... 381
Feed rate override 100 % G908 ..... 381
Interpreter stop G909 ..... 381
Spindle override 100 % G919 ..... 381
Deactivate zero-point shifts G920 ..... 382
Deactivate zero-point shifts, tool lengths G921 ..... 382
End position of tool G922 ..... 382
Fluctuating spindle speed G924 ..... 382
Convert lengths G927 ..... 383
Calculate variables automatically G940 ..... 383
Misalignment compensation G976 ..... 385
Activate zero-point shifts G980 ..... 385
Activate zero-point shifts, tool lengths G981 ..... 385
Monitoring zone G995 ..... 386
Load monitoring G996 ..... 387
Activate direct program-run continuation G999 ..... 387
Converting and mirroring G30 ..... 387
Transformations of contours G99 ..... 389
Spindle synchronization G720 ..... 390
C-angle offset G905 ..... 391
Traversing to a fixed stop G916 ..... 392
Controlled parting using lag error monitoring G917 ..... 394
Force reduction G925 ..... 395
Sleeve monitoring G930 ..... 396
Eccentric turning G725 ..... 397
Transition to eccentric G726 ..... 399
Eccentric X G727 ..... 401
4.30 Data input and data output ..... 403
"WINDOW"—Output window for variables ..... 403
"WINDOW"—Output file for variables ..... 403
"INPUT"—Input of variables ..... 403
"PRINT"—Output of # variables ..... 404
HEIDENHAIN MANUALplus 620, CNC PILOT 640
23
4.31 Programming variables ..... 405
Variable types ..... 406
Reading tool data ..... 408
Reading diagnostic bits ..... 411
Reading the current NC information ..... 412
Reading general NC information ..... 414
Reading configuration data—PARA ..... 416
Determining the index of a parameter element—PARA ..... 417
Expanded variable syntax CONST – VAR ..... 418
4.32 Conditional block run ..... 420
Program branching IF..THEN..ELSE..ENDIF ..... 420
Requesting variables and constants ..... 421
WHILE..ENDWHILE program repeat ..... 422
SWITCH..CASE—program branching ..... 423
Skip level ..... 424
4.33 Subprograms ..... 425
Subprogram call: L"xx" V1 ..... 425
Dialog texts in subprogram call ..... 426
Help graphics for subprogram calls ..... 427
4.34 M commands ..... 428
M commands for program-run control ..... 428
Machine commands ..... 429
4.35 G codes from previous controls ..... 430
Contour definitions in the machining section ..... 430
Simple turning cycles ..... 432
Thread cycles (4110) ..... 437
4.36 DINplus program example ..... 439
Example of a subprogram with contour repetitions ..... 439
4.37 Connection between geometry and machining commands ..... 442
Turning Operations ..... 442
C-axis machining—front/rear face ..... 443
C-axis machining—lateral surface ..... 443
4.38 Full-surface machining ..... 444
Fundamentals of full-surface machining ..... 444
Programming of full-surface machining ..... 445
Full-surface machining with opposing spindle ..... 446
Full-surface machining with single spindle ..... 448
24
5 Touch probe cycles ..... 451
5.1 General information on touch probe cycles (software option) ..... 452
Principle of function of touch probe cycles ..... 452
Touch probe cycles for automatic operation ..... 453
5.2 Touch probe cycles for single-point measurement ..... 455
Single-point measurement for tool compensation G770 ..... 455
Single-point measurement for zero point G771 ..... 457
Zero point C axis, single-point measurement G772 ..... 459
Zero point C-axis object center G773 ..... 461
5.3 Touch probe cycles for two-point measurement ..... 463
Two-point measurement G18 transverse G775 ..... 463
Two-point measurement G18 longitudinal G776 ..... 465
Two-point measurement G17 longitudinal G777 ..... 467
Two-point measurement G19 longitudinal G778 ..... 469
5.4 Calibrating the touch probe ..... 471
Calibrate touch probe standard G747 ..... 471
Calibrate touch probe via two points G748 ..... 473
5.5 Measuring with touch probe cycles ..... 475
Paraxial probing G764 ..... 475
Probing in C axis G765 ..... 476
Probing in two axes G766 ..... 477
Probing in two axes G768 ..... 478
Probing in two axes G769 ..... 479
5.6 Search cycles ..... 480
Find hole in C face G780 ..... 480
Find hole in C lateral surface G781 ..... 482
Find stud in C face G782 ..... 484
Find stud in C lateral surface G783 ..... 486
5.7 Circular measurement ..... 488
Circular measurement G785 ..... 488
Determine pitch circle G786 ..... 490
5.8 Angular measurement ..... 492
Angular measurement G787 ..... 492
Misalignment compensation after angle measurement G788 ..... 494
5.9 In-process measurement ..... 495
Measure workpieces (option) ..... 495
Switch on measurement G910 ..... 495
Measuring path monitoring G911 ..... 496
Measured value capture G912 ..... 496
End in-process measuring G913 ..... 496
Switch off measuring-path monitoring G914 ..... 496
In-process measurement example: Measuring and compensating workpieces ..... 497
In-process measurement example: Measuring and compensating workpieces (measure_pos_move.ncs) ..... 498
HEIDENHAIN MANUALplus 620, CNC PILOT 640
25
6 DIN programming for the Y axis ..... 499
6.1 Y-axis contours—Fundamentals ..... 500
Position of milling contours ..... 500
Cutting limit ..... 501
6.2 Contours in the XY plane ..... 502
Starting point of contour in XY plane G170-Geo ..... 502
Line segment in XY plane G171-Geo ..... 502
Circular arc in XY plane G172-Geo/G173-Geo ..... 503
Hole in XY plane G370-Geo ..... 504
Linear slot in XY plane G371-Geo ..... 505
Circular slot in XY plane G372-Geo/G373-Geo ..... 506
Full circle in XY plane G374-Geo ..... 506
Rectangle in XY plane G375-Geo ..... 507
Eccentric polygon in XY plane G377-Geo ..... 507
Linear pattern in XY plane G471-Geo ..... 508
Circular pattern in XY plane G472-Geo ..... 509
Single surface in XY plane G376-Geo ..... 510
Centric polygon in XY plane G477-Geo ..... 510
6.3 Contours in the YZ plane ..... 511
Starting point of contour in YZ plane G180-Geo ..... 511
Line segment in YZ plane G181-Geo ..... 511
Circular arc in YZ plane G182-Geo/G183-Geo ..... 512
Hole in YZ plane G380-Geo ..... 513
Linear slot in YZ plane G381-Geo ..... 513
Circular slot in YZ plane G382-Geo/G383-Geo ..... 514
Full circle in YZ plane G384-Geo ..... 514
Rectangle in YZ plane G385-Geo ..... 515
Eccentric polygon in YZ plane G387-Geo ..... 515
Linear pattern in YZ plane G481-Geo ..... 516
Circular pattern in YZ plane G482-Geo ..... 517
Single surface in YZ plane G386-Geo ..... 518
Centric polygon in YZ plane G487-Geo ..... 518
6.4 Working planes ..... 519
Y-axis machining ..... 519
G17 XY plane (front or rear face) ..... 519
G18 XZ plane (turning) ..... 519
G19 YZ plane (lateral view / lateral surface) ..... 519
Tilting the working plane G16 ..... 520
6.5 Tool positioning in the Y axis ..... 521
Rapid traverse G0 ..... 521
Approach tool change point G14 ..... 521
Rapid traverse to machine coordinates G701 ..... 521
26
6.6 Linear and circular movements in the Y axis ..... 522
Milling: Linear movement G1 ..... 522
Milling: Circular movement G2, G3—incremental center coordinates ..... 523
Milling: Circular movement G12, G13—absolute center coordinates ..... 524
6.7 Milling cycles for the Y axis ..... 525
Area milling—roughing G841 ..... 525
Area milling—finishing G842 ..... 526
Centric polygon milling—roughing G843 ..... 527
Centric polygon milling—finishing G844 ..... 528
Pocket milling—roughing G845 (Y axis) ..... 529
Pocket milling—finishing G846 (Y axis) ..... 535
Engraving in XY plane G803 ..... 537
Engraving in the YZ plane G804 ..... 538
Thread milling in XY plane G800 ..... 539
Thread milling in YZ plane G806 ..... 540
Hobbing G808 ..... 541
6.8 Example program ..... 542
Machining with the Y axis ..... 542
HEIDENHAIN MANUALplus 620, CNC PILOT 640
27
7 TURN PLUS ..... 549
7.1 TURN PLUS mode of operation ..... 550
TURN PLUS concept ..... 550
7.2 Automatic working plan generation (AWG) ..... 551
Generating a working plan ..... 551
Overview of machining sequences ..... 555
Setting the AWG control graphic ..... 563
7.3 Machining information ..... 564
Tool selection, turret assignment ..... 564
Contour recessing, recess turning ..... 566
Drilling ..... 566
Cutting data, coolant ..... 567
Inside contours ..... 567
Shaft machining ..... 570
7.4 Example ..... 572
Creating a program ..... 572
Workpiece blank definition ..... 572
Defining the basic contour ..... 573
Defining form elements ..... 573
Preparing the machining process, chucking ..... 574
Generating and saving a working plan ..... 575
7.5 Full-surface machining with TURN PLUS ..... 576
Rechucking the workpiece ..... 576
Defining the chucking equipment for full-surface machining ..... 577
Automatic program creation for full-surface machining ..... 578
Rechucking the workpiece in the main spindle ..... 578
Transferring the workpiece from the main spindle to the opposing spindle ..... 578
Parting and picking-off the workpiece with the opposing spindle ..... 579
28
8 B axis ..... 581
8.1 Fundamentals ..... 582
Tilted working plane ..... 582
8.2 Compensation with the B axis ..... 585
Compensation during program run ..... 585
8.3 Simulation ..... 586
Simulation of the tilted plane ..... 586
Displaying the coordinate system ..... 587
Position display with the B and Y axes ..... 587
HEIDENHAIN MANUALplus 620, CNC PILOT 640
29
9 Overview of units ..... 589
9.1 Units—"Turning" group ..... 590
"Roughing" group ..... 590
"Finishing" group ..... 590
"Recessing" group ..... 591
"Thread" group ..... 591
9.2 Units—"Drilling" group ..... 592
"Centric drilling" group ..... 592
"ICP drilling, C axis" group ..... 592
"C-axis face drilling" group ..... 592
"C-axis lateral surface drilling" group ..... 593
9.3 Units—"Predrilling in C axis" group ..... 594
"Predrilling in C-axis, face" group ..... 594
"Predrilling in C-axis, lateral surface" group ..... 594
9.4 Units—"Milling in C axis" group ..... 595
"Milling in C-axis, face" group ..... 595
"ICP milling in C axis, face" group ..... 595
"C-axis lateral surface milling" group ..... 596
"ICP milling in C axis, lateral surface" group ..... 596
9.5 Units—"Drilling, predrilling in Y axis" group ..... 597
"ICP drilling, Y axis" group ..... 597
"Predrilling in Y axis" group ..... 597
9.6 Units—"Milling in Y axis" group ..... 598
"Milling in front face" group (XY plane) ..... 598
"Milling in lateral surface" group (YZ plane) ..... 599
9.7 Units—"Special units" group ..... 600
30
10 Overview of G codes ..... 601
10.1 Section codes ..... 602
10.2 Overview of G commands in the CONTOUR section ..... 603
G commands for turning contours ..... 603
G commands for C-axis contours ..... 604
G commands for Y-axis contours ..... 604
10.3 Overview of G commands in the MACHINING section ..... 605
G commands for turning ..... 605
Cycles for turning ..... 606
C-axis machining ..... 607
Y-axis machining ..... 608
Variable programming, program branches ..... 608
Other G codes ..... 609
HEIDENHAIN MANUALplus 620, CNC PILOT 640
31
32
NC programming
HEIDENHAIN MANUALplus 620, CNC PILOT 640
33
1.1 smart.Turn and DIN (ISO) programming
1.1 smart.Turn and DIN (ISO)
programming
The Steuerung supports the following types of NC programming:
 Conventional DIN programming: You program the basic contour
with line segments, circular arcs and simple turning cycles. Use the
smart.Turn editor in ISO mode.
 DIN PLUS programming: The geometrical description of the
workpiece and the machining process are separated. You first
program the geometry of the blank and finished part. Then you
machine the workpiece, using contour-related turning cycles. Use
the smart.Turn editor in ISO mode.
 smart.Turn programming: The geometrical description of the
workpiece and the machining process are separated. You program
the geometry of the blank and finished part, and you program the
machining blocks as units. Use the smart.Turn editor in unit mode.
Depending on the type and complexity of your machining task, you can
use either simple DIN/ISO programming, "DIN PLUS" (ISO)
programming or smart.Turn programming. All three named
programming modes can be combined in one NC program.
In DIN PLUS and smart.Turn programming, contours can be described
with ICP interactive graphics. ICP saves the contour descriptions as G
codes in the NC program.
Parallel operation: While you are editing and testing programs, your
machine can run another NC program.
Contour follow-up
The Steuerung uses the contour follow-up function in DIN PLUS and
smart.Turn programs. The Steuerung takes the blank part as a basis
and accounts for each cut and each cycle when regenerating the
contour. Thus you can inspect the current contour of the workpiece
during each machining stage. With the "contour follow-up" function,
the Steuerung optimizes the paths for approach and departure and
avoids air cuts.
Contour regeneration is only available for turning operations when a
blank part has been programmed. It also works with auxiliary contours.
34
NC programming
1.1 smart.Turn and DIN (ISO) programming
Structured NC program
smart.Turn and DIN PLUS programs are structured in fixed sections.
The following program sections are created automatically in a new NC
program:
Beispiel: "Structured smart.Turn program"
HEADER
 Program head: Contains information on the material of the
workpiece, the unit of measure as well as further organizational data
and setup information as a comment.
 Chucking equipment: Description of the workpiece clamping
situation.
 Workpiece blank: The workpiece blank is stored. Programming a
blank activates the contour follow-up.
 Finished part: The finished part is stored. It is advisable to describe
the complete workpiece as a finished part. The units or fixed cycles
use NS and NE to indicate the workpiece section to be machined.
 Machining: Use units or cycles to program the individual machining
steps. In a smart.Turn program, the START unit is located at the
beginning of the machining process, and the END unit at the end.
 End: Indicates the end of the NC program.
#MEASURE_UNITS METRIC
If required, for example for machining with the C axis or when
programming with variables, you add further program sections.
CLAMPS 1
Use ICP (Interactive Contour Programming) for describing
blank and finished parts.
#MATERIAL
Steel
#MACHINE
Automatic lathe
#DRAWING
356_787.9
#CLAMP_PRESS.
20
#COMPANY
Turn & Co
TURRET
T1
ID"038_111_01"
T2
ID"006_151_A"
H0 D0 Z200 B20 O-100 X120 K12 Q4
BLANK
N1 G20 X120 Z120 K2
FINISHED
N2 G0 X0 Z0
N3 G1 X20 BR3
N4 G1 Z-24
...
MACHINING
N50 UNIT ID"START" [Program beginning]
N52 G26 S4000
N53 G59 Z320
N54 G14 Q0
N25 END_OF_UNIT
...
[Machining commands]
...
N9900 UNIT ID"END" [End of program]
N9902 M30
N9903 END_OF_UNIT
END
HEIDENHAIN MANUALplus 620, CNC PILOT 640
35
1.1 smart.Turn and DIN (ISO) programming
Linear and rotary axes
Principal axes: Coordinates of the X, Y and Z axes refer to the
workpiece zero point.
C axis as reference axis:
 Angle data are with given respect to the zero point of the C axis.
 C-axis contours and C-axis operations:
 Positions on the front/rear face are entered in Cartesian
coordinates (XK, YK), or polar coordinates (X, C)
 Positions on the lateral surface are entered in polar coordinates (Z,
C). Instead of C, the linear value CY can be used ("unrolled"
reference diameter).
 The smart.Turn editor respects only address letters of
the configured axes.
Units of measure
You write NC programs in metric or inch values. The unit of measure
is defined in the "Unit" box (See "HEADER section" on page 48.).
Once the unit of measure has been defined, it cannot be
edited any longer.
36
NC programming
1.1 smart.Turn and DIN (ISO) programming
Elements of an NC program
An NC program consists of the following elements:
 Program name
 Program section codes
 Units
 NC blocks
 Commands for program structuring
 Comment blocks
The program name begins with "%" followed by up to 40 characters
(numbers, uppercase letters or underscore; no diacritical marks) and
the extension "nc" for main programs or "ncs" for subprograms. The
first character must be a number or a letter.
Program section codes: When you create a new NC program, certain
program section codes are already entered. You can add new codes
or delete existing ones, depending on your program requirements. An
NC program must contain at least the MACHINING and END section
codes.
The unit begins with this keyword followed by the identification of
the unit (ID"G..."). The following lines contain the G, M and T
functions of this machining block. The unit ends with
END_OF_UNIT followed by a check digit.
NC blocks begin with an N followed by a block number (with up to five
digits). The block numbers do not affect the sequence in which the
program blocks are executed. They are only intended for identifying
the individual NC blocks.
The NC blocks of the HEADER and TURRET sections are not included
in the block number organization of the editor.
You can use program jumps, repeats and subprograms to structure
a program (example: machining the beginning/end of a bar, etc.).
Input and output: With "input" you can influence the flow of the NC
program. Using "output," you can communicate with the machinist.
Example: The machinist is required to check measuring points and
update compensation values.
Comments are enclosed in brackets "[...]." They are located at the end
of an NC block or in a separate NC block. Press the key combination
CTRL+K to convert an existing block into a comment (and vice versa).
You can also enclose more than one program line in square brackets
to mark them as a comment. To do this, enter a comment containing
the character "[" and conclude the section by entering another
comment containing the character "]".
HEIDENHAIN MANUALplus 620, CNC PILOT 640
37
1.2 The smart.Turn editor
1.2 The smart.Turn editor
Menu structure
You can select the following editor modes in the smart.Turn editor:
 Unit programming (standard)
 DIN/ISO mode (DIN PLUS and DIN 66025)
The menu structure of the smart.Turn editor is shown in the illustration
at right. Many menu items are used in both modes. The menus differ
in the area of geometry and part programming. In DIN/ISO mode the
menu items "Geo(metry)" and "Mach(ining)" are displayed instead of
the menu items "ICP" and "Units" (see illustrations at lower right). You
can switch between the editor modes by soft key.

Switches between the Unit mode and DIN/ISO mode
For special cases you can change to the text-editor mode in order to
edit character-by-character without syntax checking. The setting is
made in the Configuration / Input mode menu item.
For a description of the functions, please refer to the following
chapters:
 Shared menu items: see "Menu structure" on page 38.
 ICP functions: Chapter 5 in the User's Manual
 Units for turning and C-axis machining: see "smart.Turn units" on
page 59.
 Units for Y-axis machining: see "smart.Turn units for the Y axis" on
page 167.
 G codes for turning and C-axis machining (geometry and machining):
see "DIN Programming" on page 189.
 G codes for Y-axis machining (geometry and machining): see "DIN
programming for the Y axis" on page 501.
38
NC programming
1.2 The smart.Turn editor
Parallel editing
Up to 6 NC programs can be opened simultaneously in the smart.Turn
editor. The editor shows the names of the open programs in the tab
bar. If you have changed the NC program, the editor displays the name
in red.
You can program in the smart.Turn editor while the machine is running
a program in the automatic mode.
 The smart.Turn editor saves all open programs with
every mode change.
 The program running in the automatic mode cannot be
edited.
Screen layout
1
2
3
4
5
6
Menu bar
NC program bar with the names of the loaded NC programs. The
selected program is marked.
Program window
Contour display or large program window
Soft keys
Status bar
1
2
3
4
6
5
HEIDENHAIN MANUALplus 620, CNC PILOT 640
39
1.2 The smart.Turn editor
Selecting the editor functions
The functions of the smart.Turn editor are contained in the main menu
and various submenus.
The submenus can be called by:


selecting the desired menu item
positioning the cursor in the respective program section
Soft keys with active program window
Starts the current program in the
simulation.
Opens the contour, in which the
cursor is located, in ICP.
You can access the higher-level menu:

by pressing the ESC key
 by using the menu item
Soft keys: Soft keys are available for fast switching to "neighboring
operating modes," for changing the editing window or program view,
and for activating the graphics.
Activates the zoom function in the
contour display.
Switches between the DINplus view
and the tree view.
Switches between the Unit mode and
DIN/ISO mode.
Activates the contour display and
starts redrawing the contour.
Editing with active tree view




Press the right arrow key to expand the program sections.
Position the cursor on the program line you want to edit and press
the right arrow key once again.
The control automatically changes to the DINplus view. Make the
required changes.
Use the left arrow key to return to the tree view and to collapse the
program section.
You can adapt the tree view in the MACHINING section to
suit your requirements; for example, you can combine
multiple units to create a custom range of blocks. Define
the new range of blocks by inserting the DINplus word
BLOCKSTART at the beginning of the selected program
section and the DINplus word BLOCKEND at the end. The
DINplus words are available in the Extras menu > "Insert
DINplus word."
40
NC programming
1.2 The smart.Turn editor
Shared menu items
The menu items described below are used both in smart.Turn mode
and in DIN/ISO mode.
"Program management" pull-down menu
The "Prog" pull-down menu (program management) contains the
following functions for NC main and subprograms:
 Open: Load existing programs
 New: Create new programs
 Close: The selected program is closed
 Close All: All open programs are closed
 Save: The selected program is saved
 Save As: The selected program is saved under a new name
 Direct opening of the last four programs
When an NC program is opened or when a new NC program is
created, the soft-key row is switched to the sorting and organization
functions see "Sorting, file organization" on page 46..
"Head" pull-down menu (program head)
The "Head" pull-down menu (program head) contains functions for
editing the program head and the tool list.
 Program head: Edit the program header
 Go to chucking equipment: Positions the cursor in the "chucking
equipment" section
 Insert chucking equipment: Describe how the workpiece is
clamped
 Go to tool list: Positions the cursor in the TURRET section
 Set up the tool list: Activates the "Set up tool list" function (see
page 55)
"ICP" pull-down menu
The "ICP" pull-down menu (Interactive Contour Programming)
contains the following functions:
 Contour editing: Change the current contour (cursor position)
 Workpiece blank: Edit the description of the workpiece blank
 Finished part: Edit the description of the finished part
 New auxiliary blank: Create a new auxiliary workpiece blank
 New aux. contour: Create a new auxiliary contour
 C axis ...: Create patterns and milling contours on the front face and
lateral surface
 Y axis ...: Create patterns and milling contours in the XY and YZ
planes
HEIDENHAIN MANUALplus 620, CNC PILOT 640
41
1.2 The smart.Turn editor
"Goto" pull-down menu
The "Goto" pull-down menu contains the following jump and search
functions:
 Jump targets—The editor positions the cursor to the selected jump
target:
 To beginning
 To tool table
 To finished part
 To machining
 To end
 Search functions
 Find block number: You specify a certain block number. The
editor jumps to this block number if it exists.
 Find unit: The editor opens the list of units available in the
program. Select the desired unit.
 Find NC word: The editor opens the dialog for entering the
desired NC word. You can use the soft keys to search forward or
backward.
 Search for contour: The editor opens the list of contours
available in the program. Select the desired contour.
"Configuration" pull-down menu
The "Config" pull-down menu (Configuration) contains the following
functions:
 Input mode ...: Define the input mode
 ... NC editor (word-by-word): The editor works in the NC mode
(word by word)
 ... Text editor (character): The editor works character by
character (no syntax checking)
 Settings ...
 ... Save: The editor memorizes the open NC programs and the
respective cursor positions.
 ... Load last saved setting: Restores the last saved condition of
the editor.
 Technology data: Starts the technology editor
42
NC programming
1.2 The smart.Turn editor
"Miscellaneous" pull-down menu
The "Misc" pull-down menu (Miscellaneous) contains the following
functions:
 Insert block ...
 ... W/o block no.: The editor inserts an empty line at the cursor
position (without block number).
 ... With block no.: The editor inserts an empty line at the cursor
position (with block number). Alternative: When you press the
INS key, the editor inserts a block with block number.
 ... Comment at line end: The editor inserts a comment at the end
of the line in which the cursor is located.
 Edit word: You can edit the NC word at which the cursor is located.
 Delete word: The editor deletes the NC parameter at the cursor
position.
 Dissolve unit: Position the cursor to the first line of a unit before
selecting this menu item. The editor cancels the brackets around
the unit. The unit dialog can no longer be used for this machining
block, but you can edit the machining block as desired.
 Block numbering: The block numbering settings are the starting
block number and the block-number increment. The first NC block
receives the starting block number and the block-number increment
is added for each further NC block. The settings for starting block
number and block-number increment are tied with the NC program.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
43
1.2 The smart.Turn editor
"Extras" pull-down menu
The "Extras" pull-down menu contains the following functions:
 DIN PLUS word: The editor opens the selection list with all DIN
PLUS words in alphabetical order. Select the desired instruction for
program structuring or the input/output command. The editor
inserts the DIN PLUS word at the cursor position.
 Comment line: The comment is inserted above the position of the
cursor.
 Constant definition: The expression is inserted above the position
of the cursor. If the DIN PLUS word "CONST" is not present yet, it is
also inserted.
 Assignment of variables: Inserts a variable instruction.
 L call external (the subprogram is in a separate file): The editor
opens the file selection window for subprograms. Select the
subprogram and fill out the subprogram dialog. The control searches
for subprograms in the sequence: current project, standard directory
and then machine manufacturer directory.
 L call internal (the subprogram is contained in the main program):
The editor opens the subprogram dialog.
 Block functions. This pull-down menu contains functions for
marking, copying and deleting sections.
 Marking On/Off: Activates/Deactivates the marking mode during
cursor movement.
 Cancel marking: After calling the menu item, no part of the
program is marked.
 Cut: Deletes the marked part of the program and copies it to the
clipboard.
 Copy: Copies the marked part of the program into the clipboard.
 Insert: Inserts the contents of the clipboard at the cursor position.
Any parts of the program that are marked are replaced by the
contents of the clipboard.
44
NC programming
1.2 The smart.Turn editor
"Graphics" pull-down menu
The "Graph." pull-down menu contains the following functions (see
figure at right):
 Graphic ON: Activates the graphic window or updates the
displayed contour. As an alternative, you can use the soft key (see
table at right).
 Graphic OFF: Closes the graphic window.
 Graphic for Automatic: The graphic window is activated when the
cursor is located in the contour description.
 Window: Sets the graphic window. During editing, the Steuerung
displays programmed contours in up to four graphic windows. Set
the desired windows.
 Magnifier on: Activates the zoom function. As an alternative, you
can use the soft key (see table at right).
The graphic window:
 Colors in contour graphics:
 White: workpiece blank and auxiliary blank
 Yellow: finished part
 Blue: auxiliary contours
 Red: contour element at the current cursor position. The arrow
point indicates the direction of machining.
 When programming fixed cycles, you can use the displayed contour
for establishing block references.
 Using the zoom functions, you can magnify, reduce or shift details.
Soft keys with active program window
Activates the contour display and
starts redrawing the contour.
Opens the soft-key menu for the
zoom functions and displays the zoom
frame.
 Additions/changes to the contour will not be considered
until the GRAPHICS soft key is pressed again.
 Unambiguous NC block numbers are a prerequisite for
the contour display!
HEIDENHAIN MANUALplus 620, CNC PILOT 640
45
1.2 The smart.Turn editor
Sorting, file organization
When an NC program is opened or when a new NC program is
created, the soft-key row is switched to the sorting and organization
functions. Use the soft keys to select the order in which the programs
are to be displayed, or use the functions for copying, deleting, etc.
Soft keys file manager
Deletes the selected program after confirmation
prompt
Makes it possible to change the program name
Copies the selected program
Switches the write protection attribute on or off for the
selected program
Activates the alphabetic keyboard
Soft keys for sorting
Displays the file attributes: size, date, time
Sorts by file name
Sorts by file size
Sorts by creation date or change date
Reverses the sorting direction
Opens the selected program
46
NC programming
1.3 Program section code
1.3 Program section code
A new NC program is already provided with section codes. You can
add new codes or delete existing ones, depending on your program
requirements. An NC program must contain at least the MACHINING
and END section codes.
Further program section codes are available in the "Insert DIN PLUS
word" selection list ("Extras > DIN PLUS word" menu item). The
Steuerung enters the program section code at the correct position or
at the current position.
German program section codes are used when German is set as the
conversational language. All other languages use English program
section codes.
Overview of program section codes
German
English
Program head
PROGRAMMKOPF
HEADER
Page 48
SPANNMITTEL
CLAMPS
Page 49
REVOLVER
TURRET
Page 50
ROHTEIL
BLANK
Page 50
FERTIGTEIL
FINISHED
Page 50
HILFSKONTUR
AUXIL_CONTOUR
Page 50
HILFSROHTEIL
AUXIL_BLANK
Page 50
Beispiel: Program section codes
...
[Sections of the contour description]
BLANK
N1 G20 X100 Z220 K1
Contour definition
FINISHED
N2 G0 X60 Z0
N3 G1 Z-70
...
FACE_C Z-25
N31 G308 ID"01" P-10
C-axis contours
STIRN
FACE_C
Page 51
RUECKSEITE
REAR_C
Page 51
MANTEL
LATERAL_C
Page 51
N32 G402 Q5 K110 A0 Wi72 V2 XK0 YK0
N33 G300 B5 P10 W118 A0
N34 G309
FACE_C Z0
Y-axis contours
N35 G308 ID"02" P-6
STIRN_Y
FACE_Y
Page 51
RUECKSEITE_Y
REAR_Y
Page 51
N37 G309
MANTEL_Y
LATERAL_Y
Page 52
...
BEARBEITUNG
MACHINING
Page 53
ENDE
END
Page 53
N36 G307 XK0 YK0 Q6 A0 K34.641
Workpiece machining
HEIDENHAIN MANUALplus 620, CNC PILOT 640
47
1.3 Program section code
Overview of program section codes
German
English
Subprograms
UNTERPROGRAMM
SUBPROGRAM
Page 53
RETURN
RETURN
Page 53
CONST
CONST
Page 54
VAR
VAR
Page 54
Others
For more than one independent contour definition for
drilling/milling, use the program section codes (FACE_C,
LATERAL_C, etc.) each time.
HEADER section
Instructions and information in the program head (HEADER):
 Unit:
 Select dimensional system in millimeters or inches
 No entry: The unit set in the user parameter is used
 The other fields contain organizational information and set-up
information, which do not influence the machining process.
Information contained in the program head is preceded by "#" in the NC
program.
You can only select a unit when creating a new NC
program. It is not possible to post-edit this entry.
48
NC programming
1.3 Program section code
CLAMPS section
In the CLAMPS program section you describe how the workpiece is
clamped. This makes it possible to display the chucking equipment
during simulation. In TURN PLUS the chucking equipment information
is used to calculate the zero points and cutting limits during automatic
program generation.
Parameters
H
Chuck number
D
Spindle number for AWG
R
Clamp type
O
I
K
X
Q
 0: Parameter J defines the free length
 1: Parameter J defines the clamping length
Position of the chuck edge
Chuck jaw reference
Clamping length or free length of the workpiece (depending
on the clamp type R)
Cutting limit for outside machining
Cutting limit for inside machining
Overlap jaw/workpiece (pay attention to sign)
Clamping diameter of workpiece blank
Chuck form
V
 4: Outside chucking
 5: Inside chucking
Shaft machining AWG
Z
B
J
 0: Chuck: Automatic separation points at largest and
smallest diameter
 1: Shaft/chuck: Machining also starting from the chuck
 2: Shaft/face driver: Outside contour can be machined
completely
If you do not define the parameters Z and B, TURN PLUS
will use the following machine parameters (see "List of
user parameters" in the User's Manual) during AWG
(automatic working plan generation):
 Front chuck edge on spindle / counterspindle
 Jaw width on spindle / counterspindle
HEIDENHAIN MANUALplus 620, CNC PILOT 640
49
1.3 Program section code
TURRET section
The TURRET program section defines the assignment of the tool
carrier. For every assigned turret pocket, the tool ID number is
entered. For multipoint tools, every cutting edge is entered in the
turret list.
 If you do not program the TURRET, the tools entered
in the tool list of the Machine operating mode will be
used.
Beispiel: Turret table
...
TURRET
T1 ID"342-300.1"
T2 ID"C44003"
...
BLANK section
In this program section, you describe the contour of the workpiece
blank.
AUXIL_BLANK section
In the AUXIL_ BLANK section, you define additional workpiece blanks,
which can be activated with G702 when required.
FINISHED section
In this program section, you describe the contour of the finished part.
After the FINISHED section you use additional section codes such as
FACE_C, LATERAL_C, etc.
AUXIL_CONTOUR section
In this program section, you describe the auxiliary turning contours.
50
NC programming
1.3 Program section code
FACE_C, REAR_C sections
In this program section you describe the front and rear side contours
to be machined with the C axis. The program section defines the
position of the contour in Z direction.
Parameter
Z
Position of the front/rear-face contour
LATERAL_C section
In this program section you describe the lateral surface contours to be
machined with the C axis. The program section defines the position of
the contour in X direction.
Parameter
X
Reference diameter of the lateral-surface contour
FACE_Y, REAR_Y sections
For lathes with Y axis, these program section codes define the XY
plane (G17) and the position of the contour in Z direction. The spindle
angle (C) defines the spindle position.
Parameters
X
Area diameter (as cutting limit)
Z
Position of the reference plane—default: 0
C
Spindle angle—default: 0
HEIDENHAIN MANUALplus 620, CNC PILOT 640
51
1.3 Program section code
LATERAL_Y section
The section code identifies the YZ plane (G19). For machines equipped
with a B axis, it defines the tilted plane.
B, I, K
Without tilted plane: The reference diameter defines the contour
position in the X direction; the C-axis angle defines the position on the
workpiece.
–I
X
Parameters
X
Reference diameter
C
H=0
B
H=1
I
C axis angle—Defines the spindle position
Z
–K
With tilted plane (see figures): LATERAL_Y additionally performs the
following transformations and rotations for the tilted plane:
 Shifts the coordinate system to the position I, K
 Rotates the coordinate system by the angle B; reference point: I, K
 H=0: Shifts the rotated coordinate system by –I. The coordinate
system is moved "back."
Parameters
X
Reference diameter
C
C axis angle—Defines the spindle position
B
Plane angle: Positive Z axis
I
Plane reference in X direction (radius)
K
Plane reference in Z direction
H
Automatic shift of the coordinate system (default: 0)
X
X
B
B
Z
Z
 0: The rotated coordinate system is shifted by –I
 1: The coordinate system is not shifted
Shifting "back" the coordinate system: The control evaluates the
reference diameter for the cutting limit. This value is also used as the
reference value for the depth that you program for drilling operations
and milling contours.
Since the reference diameter is referenced to the current zero point,
it is recommended when working in a tilted plane, to shift the rotated
coordinate system "back" by the distance –I. If the cutting limits are not
needed, for example for drilling holes, you can disable the shift of the
coordinate system (H=1) and set the reference diameter to 0.
52
Beispiel: LATERAL_Y
HEADER
...
CONTOUR Q1 X0 Z600
BLANK
...
FINISHED
Please note:
...
 X is the infeed axis in a tilted coordinate system. X
coordinates are entered as diameter coordinates.
 Mirroring the coordinate system has no effect on the
reference axis of the tilt angle ("B axis angle" of the tool
call).
LATERAL_Y X118 C0 B130 I59 K0
...
MACHINING
...
NC programming
1.3 Program section code
MACHINING section
In the MACHINING program section you program the machining
operations. This code must be included.
END code
The END code concludes the NC program. This code must be included.
SUBPROGRAM section
If you define a subprogram within your NC program (within the same
file), it is designated with SUBPROGRAM, followed by the name of the
subprogram (max. 40 characters).
RETURN code
The RETURN code concludes the subprogram.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
53
1.3 Program section code
CONST code
In the CONST section of the program you define constants. You use
constants for the definition of a value.
You enter the value directly or you calculate it. If you use constants in
the calculation you must first define them.
The length of the constant name must not exceed 20 characters.
Lower case letters and numbers are allowed. Constants always begin
with an underscore: see "Expanded variable syntax CONST – VAR" on
page 420.
Beispiel: CONST
CONST
_nvr = 0
_sd=PARA("","CfgGlobalTechPara","safetyDis
tWorkpOut")
_nws = _sd-_nvr
...
BLANK
N 1 G20 X120 Z_nws K2
...
MACHINING
N 6 G0 X100+_sd
...
VAR code
In the VAR program section, you assign names (descriptive text) to
variables: see "Expanded variable syntax CONST – VAR" on page 420.
The length of the variable name must not exceed 20 characters. Lower
case letters and numbers are allowed. Variables always begin with "#".
Beispiel: VAR
VAR
#_inside_dm = #l2
#_length = #g3
...
BLANK
N 1 #_length=120
N 2 #_inside_dm=25
N 3 G20 X120 Z#_length+2 K2 I#_inside_dm
...
MACHINING
...
54
NC programming
1.4 Tool programming
1.4 Tool programming
The designations of the tool pockets are fixed by the machine tool
builder. Each tool holder has a unique T number.
In the T command (MACHINING section) you program the T number,
and therefore the position to which the tool carrier rotates. The
Steuerung retrieves the assignment of the tools to the turret position
from the turret list of the TURRET section.
You can edit the tool entries individually, or you can call the tool list via
the Set up the turret list menu item and then edit it.
Setting up a tool list
In the "Set up the turret list" function, the Steuerung provides the turret
assignment as a tool list for editing.
You have the following options:
 Editing the turret assignment: Transfer tools from the database,
delete entries or move them to other positions (for soft keys see
table).
 Loading the turret list of the Machine mode of operation.
 Deleting the current turret assignment of the NC program.
Loading the turret list of the Machine mode of operation:

Select "Head > Set up the turret list."
 Switch to "Special functions."

Load the tool list of the Machine mode of operation
into the NC program.
Deleting a tool list:

Select "Head > Set up the turret list."
 Switch to "Special functions."

Delete all entries of the turret list.
Soft keys in turret list
Delete entry
Paste entry from clipboard
Cut out entry and save it in the clipboard
Show entries in the tool database
Save the turret assignment
Close the tool list. You decide whether
the changes made remain in effect
The input window of the selected tool is
opened for editing
HEIDENHAIN MANUALplus 620, CNC PILOT 640
55
1.4 Tool programming
Editing tool entries
For each entry of the TURRET section you call the Tool dialog box,
enter the identification number or use the identification number from
the tool database.
New tool entry
Position the cursor and press the INS (insert) key. The
editor opens the Tool dialog box.
Enter the identification number of the tool.
Open the tool database.
Place the cursor on the tool to be loaded.
Transfer the identification number of the tool.
Parameters of the "Tool" dialog box
T number
Position on tool carrier
ID number
ID number (reference to
database)
Editing the tool data
Position the cursor on the entry to be edited and press RETURN.
Replacement tool Identification number of the
tool to be used when the
previous tool is worn out.
Edit the Tool dialog box.
Replacement
strategy
 0: Complete tool
 1: Secondary cutting edge or
any
Multipoint tools
A multipoint tool is a tool with multiple reference points or multiple
cutting edges. During T call, the T number is followed by an S to
identify the cutting edge.
T number.S (S=0 to 9)
S=0 identifies the main cutting edge, which does not need to be
programmed.
Examples:
 T3 or T3.0: Tilted position 3; main cutting edge
 T12.2: Tilted position 12; cutting edge 2
56
NC programming
1.4 Tool programming
Replacement tools
During "simple" tool life monitoring the control stops program run
when a tool is worn out. However, the program run is then resumed
and concluded.
If you use the tool life monitoring with replacement tools function,
the Steuerung automatically inserts the "sister tool" as soon as the tool
is worn out. The Steuerung does not stop the program run until the
last tool of the tool sequence of exchange is worn out.
You can define replacement tools when setting up the turret. The
"interchange chain" can contain more than one replacement tool. The
interchange chain is a part of the NC program.
In the T commands, you program the first tool to be changed.
Defining replacement tools
Place the cursor on the previous tool and press RETURN.
Enter the identification number of the replacement tool (Tool dialog
box) and define the replacement strategy.
When using multipoint tools, you define in the replacement strategy
whether the complete multipoint tool or only the worn-out cutting
edge of the tool is to be replaced by a replacement tool:
 0: Complete tool (default): If a cutting edge of the multipoint tool is
worn out, the tool will no longer be used.
 1: Secondary cutting edge or any: Only the worn-out cutting edge of
the multipoint tool is replaced by another tool or another cutting
edge. Any other cutting edges of the multipoint tool that are not
worn out will continue to be used.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
57
58
NC programming
1.4 Tool programming
smart.Turn units
2.1 smart.Turn units
2.1 smart.Turn units
"Units" menu
The "Units" menu contains the unit calls grouped by the type of
machining operation. Select the Units menu to call the following pulldown menus:
 Roughing
 Recessing
 Drilling and predrilling (C axis and Y axis)
 Finishing
 Thread
 Milling (C axis and Y axis)
 Special operations
The smart.Turn unit
A unit describes a complete working block. This means that the unit
includes the tool call, the technology data, the cycle call, the approach
and departure strategies as well as global data, such as safety
clearance, etc. All of these parameters are collected in one, clearly
structured dialog box.
Unit forms
The unit dialog is divided into fillable forms and the forms are divided
again into groups. You can navigate between the forms and groups
with the smart keys.
Forms in unit dialogs
Overview
Overview form with all necessary settings
Tool
Tool form with tool selection, technological settings and
M functions
Contour
Description or selection of the contour to be machined
Cycle
Description of the machining operation
Global
View and settings of globally set values
AppDep
Definition of approach and departure behavior
ToolExt
Extended tool settings
60
smart.Turn units
2.1 smart.Turn units
The Overview form
The overview form summarizes the most important settings of the
unit. These parameters are repeated in the other forms.
The Tool form
You program the technological information in this form.
Tool form
Tool
T
Tool number (number of turret pocket).
TID
The identification number (tool name) is entered
automatically.
F
Feed rate: Feed rate in revolutions for machining (mm/rev).
The tool is moved at the programmed value for each spindle
revolution.
S
(Constant) cutting speed (m/min) or constant shaft speed
(rev/min). Switchable with Type of turning GS.
Spindle
GS
Type of turning
MD
 G96: Constant surface speed. The rotational speed
changes with the turning diameter.
 G97: Constant shaft speed. Rotational speed is
independent of the turning diameter.
Direction of rotation
 M03: Clockwise (CW)
 M04: Counterclockwise (CCW)
SPI
Workpiece spindle number (0 to 3). Spindle that is holding
the workpiece (only on machines with more than one
spindle).
SPT
Tool spindle number (0 to 3). Spindle of the driven tool.
M functions
MT
M after T: M function that is executed after the tool call T.
MFS
M at beginning: M function that is executed at the beginning
of the machining step.
MFE
M at end: M function that is executed at the end of the
machining step.
Soft keys in the tool form
Selects the tool number
Loads the feed rate, cutting speed and
infeed from the technology database.
A machining operation is assigned to each unit for access
to the technology database. The following description
shows the assigned machining mode and the unit
parameters that were changed by the technology
proposal.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
61
2.1 smart.Turn units
The Contour form
In the contour form you define the contours to be machined. A
difference is made between the direct contour definition (G80) and the
reference to an external contour definition (FINISHED or
AUXIL_CONTOUR program sections).
ICP contour definition parameters
FK
Auxiliary contour: Name of the contour to be machined
NS
NE
You can select an existing contour or describe a new contour
with ICP.
Contour start block number: Beginning of contour section
Contour end block number: End of contour section
V
 NE not programmed: The contour element NS is machined
in the direction of contour definition.
 NS=NE programmed: The contour element NS is
machined opposite to the direction of contour definition.
Machine form elements (default: 0)
A chamfer/rounding arc is machined:
 0: At start and end of the contour
 1: At start of the contour
 2: At end of the contour
 3: No machining
 4: Only chamfer/rounding is machined—not the basic
element. (Requirement: the contour section consists of a
single element)
XA, ZA Starting point of blank (only effective if no blank was
programmed):
BP
BF
 XA, ZA not programmed: The workpiece blank contour is
calculated from the tool position and the ICP contour.
 XA, ZA programmed: Definition of the corner point of the
workpiece blank.
Break duration: Time span for interruption of the feed. The
chip is broken by the (intermittent) interruption of the feed.
Feed duration: Time interval until the next break. The chip is
broken by the (intermittent) interruption of the feed.
The listed soft keys are only selectable if the input cursor
is in the FK field, or on NS or NE.
Soft keys in the ICP contour form
Opens the selection list of the contours
defined in the program.
Shows all contours in the graphics
window. Use the arrow keys for
selection.
Starts the ICP editor. First, enter the
desired contour name in FK.
Starts the ICP editor with the currently
selected contour.
Opens the graphics window for
selection of a part of a contour for NS
and NE.
62
smart.Turn units
2.1 smart.Turn units
Direct contour definition parameters for turning operations
EC
Type of contour
 0: Normal contour
 1: Plunging contour
X1, Z1 Contour starting point
X2, Z2 Contour end point
RC
Rounding: Radius of contour corner
AC
Start angle: Angle of the first contour element
(range: 0° < 90°)
WC
End angle: Angle of the last contour element
(range: 0° < 90°)
BS
–Chamfer/+radius at start:
BE
BP
BF
 BS>0: Radius of rounding arc
 BS<0: Section length of chamfer
–Chamfer/+radius at end:
 BE>0: Radius of rounding arc
 BE<0: Section length of chamfer
Break duration: Time span for interruption of the feed. The
chip is broken by the (intermittent) interruption of the feed.
Feed duration: Time interval until the next break. The chip is
broken by the (intermittent) interruption of the feed.
Direct contour definition parameters for recessing operations
X1, Z1 Contour starting point
X2, Z2 Contour end point
RC
Rounding: Radii in the recess base
AC
Start angle: Angle of the first contour element
(range: 0° <= 90°)
WC
End angle: Angle of the last contour element
(range: 0° <= 90°)
BS
–Chamfer/+radius at start:
BE
 BS>0: Radius of rounding arc
 BS<0: Section length of chamfer
–Chamfer/+radius at end:
 BE>0: Radius of rounding arc
 BE<0: Section length of chamfer
HEIDENHAIN MANUALplus 620, CNC PILOT 640
63
2.1 smart.Turn units
The Global form
This form contains parameters that were defined as default values in
the start unit. You can edit these parameters in the machining units.
Parameters on the Global form
G14
Tool change point
CLT
G47
SCK
SCI
G60
 No axis
 0: Simultaneously
 1: First X, then Z
 2: First Z, then X
 3: Only X
 4: Only Z
 5: Only Y direction
 6: Simultaneous with Y (X, Y and Z axes move on a
diagonal path)
Coolant
 0: Without
 1: Circuit 1 on
 2: Circuit 2 on
Safety clearance: Indicates the distance to the current blank
material at which the tool is not moved at rapid traverse
during turning operations.
Safety clearance in infeed direction: Safety clearance in
infeed direction during drilling and milling operations.
Safety clearance in plane: Safety clearance in the working
plane during drilling and milling operations.
Protection zone. During drilling and boring the protection
zone monitoring is
 0: Active
 1: Inactive
The units G840 "Contour milling, figures" and G84X
"Pocket milling, figures" additionally provide the parameter
RB "Retraction plane" on the Global form.
64
smart.Turn units
2.1 smart.Turn units
The AppDep form
Positions and variants of the approach and departure movements are
defined in this form.
Approach: Influence the approach strategy.
"Approach" parameters
APP
Type of approach:
 No axis (switch off the approach function)
 0: Simultaneous (X and Z axes approach diagonally)
 1: First X, then Z
 2: First Z, then X
 3: Only X
 4: Only Z
XS, ZS Approach position: Position of the tool point before cycle
call
Additionally with C-axis operations:
CS
Approach position: C-axis position that is approached
before cycle call with G110.
"Approach with Y axis" parameters
APP
Type of approach:
XS, YS,
ZS
CS
 No axis (switch off the approach function)
 0: Simultaneous (X and Z axes approach diagonally)
 1: First X, then Z
 2: First Z, then X
 3: Only X
 4: Only Z
 5: Only Y direction
 6: Simultaneous with Y (X, Y and Z axes approach
diagonally)
Approach position: Position of the tool point before cycle
call
Approach position: C-axis position that is approached
before cycle call with G110.
Departure: Influence the departure strategy (also applies for Y-axis
functions).
"Departure" parameters
DEP
Type of departure:
 No axis (switch off the departure function)
 0: Simultaneous (X and Z axes depart diagonally)
 1: First X, then Z
 2: First Z, then X
 3: Only X
 4: Only Z
XE, ZE Departure position: Position of the tool point before the
movement to the tool change point.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
65
2.1 smart.Turn units
The Tool Ext form
In this form you can program additional tool settings.
Tool Ext form
Tool
T
Tool number (number of turret pocket).
TID
The identification number (tool name) is entered
automatically.
B axis
B
Angle in the B axis (machine-dependent function)
CW
C tilting plane angle: Position of the C axis to determine the
work position of the tool (machine-dependent function)
Miscellaneous functions
HC
Shoe brake (machine-dependent function)
 0: Automatic
 1: Tighten
 2: Don't tighten
DF
Additional function: Can be evaluated by the machine
manufacturer in a subprogram (machine-dependent
function)
XL, ZL, Values can be evaluated by the machine manufacturer in a
YL
subprogram (machine-dependent function)
With the Advanced T change soft key you can switch
quickly and easily between the Tool and Tool Ext forms.
66
smart.Turn units
2.2 Units—Roughing
2.2 Units—Roughing
"Longitudinal roughing in ICP" unit
The unit machines the contour described in the FINISHED program
section from "NS to NE". Any auxiliary contour defined in FK will be
used.
Unit name: G810_ICP / Cycle: G810 (see page 272)
Contour form: see page 62
Cycle form
I, K
Oversize in X, Z direction (I: diameter value)
P
Maximum infeed
E
Plunging behavior
Q
 E=0: Descending contours are not machined
 E>0: Plunging feed rate for declining contour elements.
Descending contour elements are machined.
 No input: The plunging feed rate is reduced during
machining of declining contour elements by up to 50 %.
Descending contour elements are machined.
Cutting limit (SX: diameter value)—(default: no cutting limit)
Approach angle (reference: Z axis)—(default: parallel
to Z axis)
Departure angle (reference: Z axis)—(default: orthogonal
to Z axis)
Type of retraction at end of cycle
H
 0: Returns to starting point (first X, then Z direction)
 1: Positions in front of the finished contour
 2: Retracts to safety clearance and stops
Contour smoothing
D
U
 0: With each cut along the contour (within the infeed
range)
 1: Contour smoothing with the last cut (entire contour);
retracts at 45°
 2: No smoothing; retracts at 45°
Omit elements (see figure)
Cut line on horizontal element:
O
 0: No (regular proportioning of cuts)
 1: Yes (may result in irregular proportioning of cuts)
Hide undercutting:
SX, SZ
A
W
 0: Undercuts are machined
 1: Undercuts are not machined
Further forms: see page 60
Access to the technology database:
 Machining operation: Roughing
 Affected parameters: F, S, E, P
HEIDENHAIN MANUALplus 620, CNC PILOT 640
67
2.2 Units—Roughing
"Transverse roughing in ICP" unit
The unit machines the contour described in the FINISHED program
section from "NS to NE". Any auxiliary contour defined in FK will be
used.
Unit name: G820_ICP / Cycle: G820 (see page 275)
Contour form: see page 62
Cycle form
I, K
Oversize in X, Z direction (I = diameter value)
P
Maximum infeed
E
Plunging behavior
Q
 E=0: Descending contours are not machined
 E>0: Plunging feed rate for declining contour elements.
Descending contour elements are machined.
 No input: The plunging feed rate is reduced during
machining of declining contour elements by up to 50 %.
Descending contour elements are machined.
Cutting limit (SX: diameter value)—(default: no cutting limit)
Approach angle (reference: Z axis)—(default: orthogonal
to Z axis)
Departure angle (reference: Z axis)—(default: parallel
to Z axis)
Type of retraction at end of cycle
H
 0: Returns to starting point (first X, then Z direction)
 1: Positions in front of the finished contour
 2: Retracts to safety clearance and stops
Contour smoothing
D
U
 0: With each cut along the contour (within the infeed
range)
 1: Contour smoothing with the last cut (entire contour);
retracts at 45°
 2: No smoothing; retracts at 45°
Omit elements; do not machine form elements (see figure)
Cut line on horizontal element:
O
 0: No (regular proportioning of cuts)
 1: Yes (may result in irregular proportioning of cuts)
Hide undercutting:
SX, SZ
A
W
 0: Undercuts are machined
 1: Undercuts are not machined
Further forms: see page 60
Access to the technology database:
 Machining operation: Roughing
 Affected parameters: F, S, E, P
68
smart.Turn units
2.2 Units—Roughing
"Contour-parallel roughing in ICP" unit
The unit machines the contour described in the FINISHED program
section from "NS to NE" parallel to the contour. Any auxiliary contour
defined in FK will be used.
Unit name: G830_ICP / Cycle: G830 (see page 278)
Contour form
J
Workpiece blank oversize (radius value)—active only if no
blank has been defined.
B
Contour calculation
 0: Automatic
 1: Tool to the left (G41)
 2: Tool to the right (G42)
Further parameters of the contour form: see page 62
Cycle form
P
Maximum infeed
I, K
Oversize in X, Z direction (I: diameter value)
SX, SZ Cutting limit (SX: diameter value)—(default: no cutting limit)
A
Approach angle (reference: Z axis)—(default: parallel to Z
axis)
W
Departure angle (reference: Z axis)—(default: orthogonal to
Z axis)
Q
Type of retraction at end of cycle
H
 0: Returns to starting point (first X, then Z direction)
 1: Positions in front of the finished contour
 2: Retracts to safety clearance and stops
Type of cut lines (cutting paths)
D
HR
 0: Constant cutting depth: Contour is shifted by a
constant infeed value (paraxial)
 1: Equidistant cutting lines: Cutting lines run at a constant
distance from the contour (contour parallel). The contour
is scaled.
Omit elements; do not machine form elements (see figure)
Main machining direction
 0: Automatic
 1: +Z
 2: +X
 3: -Z
 4: -X
Further forms: see page 60
Access to the technology database:
 Machining operation: Roughing
 Affected parameters: F, S, E, P
HEIDENHAIN MANUALplus 620, CNC PILOT 640
69
2.2 Units—Roughing
"Bidirectional roughing in ICP" unit
The unit machines the contour described in the FINISHED program
section from "NS to NE" parallel to the contour and bidirectionally. Any
auxiliary contour defined in FK will be used.
Unit name: G835_ICP / Cycle: G835 (see page 281)
Contour form
J
Workpiece blank oversize (radius value)—active only if no
blank has been defined.
B
Contour calculation
 0: Automatic
 1: Tool to the left (G41)
 2: Tool to the right (G42)
Further parameters of the contour form: see page 62
Cycle form
P
Maximum infeed
I, K
Oversize in X, Z direction (I = diameter value)
SX, SZ Cutting limit (SX: diameter value)—(default: no cutting limit)
A
Approach angle (reference: Z axis)—(default: parallel to Z
axis)
W
Departure angle (reference: Z axis)—(default: orthogonal to
Z axis)
Q
Type of retraction at end of cycle
H
 0: Returns to starting point (first X, then Z direction)
 1: Positions in front of the finished contour
 2: Retracts to safety clearance and stops
Type of cut lines (cutting paths)
 0: Constant cutting depth: Contour is shifted by a
constant infeed value (paraxial)
 1: Equidistant cutting lines: Cutting lines run at a constant
distance from the contour (contour parallel). The contour
is scaled.
D
Omit elements; do not machine form elements (see figure)
Further forms: see page 60
Access to the technology database:
 Machining operation: Roughing
 Affected parameters: F, S, E, P
70
smart.Turn units
2.2 Units—Roughing
"Longitudinal roughing with direct contour
input" unit
The unit machines the contour defined by the parameters. In EC you
define whether you want to machine a normal or a plunging contour.
Unit name: G810_G80 / Cycle: G810 (see page 272)
Contour form
EC
Type of contour
BS
 0: Normal contour
 1: Plunging contour
Contour starting point
Contour end point
Rounding: Radius of contour corner
Start angle: Angle of the first contour element
(range: 0° < 90°)
End angle: Angle of the last contour element
(range: 0° < 90°)
–Chamfer/+radius at start:
BE
 BS>0: Radius of rounding arc
 BS<0: Section length of chamfer
–Chamfer/+radius at end
X1, Z1
X2, Z2
RC
AC
WC
 BE>0: Radius of rounding arc
 BE<0: Section length of chamfer
BP
Break duration: Time span for interruption of the feed for
chip breaking.
BF
Feed duration: Time interval until the next break. The
interruption of the feed rate breaks the chip.
Cycle form
P
Maximum infeed
I, K
Oversize in X, Z direction (I: diameter value)
E
Plunging behavior
H
 E>0: Plunging feed rate for declining contour elements.
Descending contour elements are machined.
 No input: The plunging feed rate is reduced during
machining of declining contour elements by up to 50 %.
Descending contour elements are machined.
Contour smoothing
 0: With each cut along the contour (within the infeed
range)
 1: Contour smoothing with the last cut (entire contour);
retracts at 45°
 2: No smoothing; retracts at 45°
Further forms: see page 60
HEIDENHAIN MANUALplus 620, CNC PILOT 640
Access to the technology database:
 Machining operation: Roughing
 Affected parameters: F, S, E, P
71
2.2 Units—Roughing
"Transverse roughing with direct contour input"
unit
The unit machines the contour defined by the parameters. In EC you
define whether you want to machine a normal or a plunging contour.
Unit name: G820_G80 / Cycle: G820 (see page 275)
Contour form
EC
Type of contour
BS
 0: Normal contour
 1: Plunging contour
Contour starting point
Contour end point
Rounding: Radius of contour corner
Start angle: Angle of the first contour element
(range: 0° < AC < 90°)
End angle: Angle of the last contour element
(range: 0° < WC < 90°)
Chamfer/radius at start
BE
 BS>0: Radius of rounding arc
 BS<0: Section length of chamfer
Chamfer/radius at end
X1, Z1
X2, Z2
RC
AC
WC
 BE>0: Radius of rounding arc
 BE<0: Section length of chamfer
BP
Break duration: Time span for interruption of the feed. The
chip is broken by the (intermittent) interruption of the feed.
BF
Feed duration: Time interval until the next break. The chip
is broken by the (intermittent) interruption of the feed.
Cycle form
P
Maximum infeed
I, K
Oversize in X, Z direction (I: diameter value)
E
Plunging behavior
H
 E>0: Plunging feed rate for declining contour elements.
Descending contour elements are machined.
 No input: The plunging feed rate is reduced during
machining of declining contour elements by up to 50 %.
Descending contour elements are machined.
Contour smoothing
 0: With each cut along the contour (within the infeed
range)
 1: Contour smoothing with the last cut (entire contour);
retracts at 45°
 2: No smoothing; retracts at 45°
Further forms: see page 60
72
Access to the technology database:
 Machining operation: Roughing
 Affected parameters: F, S, E, P
smart.Turn units
2.3 Units—Recessing
2.3 Units—Recessing
"ICP contour recessing" unit
The unit machines the contour described in the FINISHED program
section axially/radially from "NS to NE". Any auxiliary contour defined
in FK will be used.
Unit name: G860_ICP / Cycle: G860 (see page 283)
Contour form
DQ
Number of recessing cycles
DX, DZ Distance to subsequent recess in X, Z direction (DX: radius
value)
Further parameters of the contour form: see page 62
Cycle form
I, K
Oversize in X, Z direction (I: diameter value)
SX, SZ Cutting limit (SX: diameter value)—(default: no cutting limit)
ET
Recessing depth by which one cut is fed.
P
Recessing width (default: 0.8 x tool width)
E
Finishing feed rate. Differing feed rate used only for the
finishing process.
EZ
Period of dwell after recessing path (default: time for one
spindle revolution)
Q
Roughing/finishing (process variants)
H
 0 (SS): Roughing and finishing
 1 (SP): Only roughing
 2 (SL): Only finishing
Type of retraction at end of cycle
 0: Return to starting point
 Axial recess: First Z, then X direction
 Radial recess: First X, then Z direction
O
 1: Positions in front of the finished contour
 2: Retracts to safety clearance and stops
End of rough cut
U
 0: Lift-up at rapid
 1: Half recessing width 45°
End of finishing cut
Access to the technology database:
 Machining operation: Contour recessing
 Affected parameters: F, S, E
 0: Value from global parameter
 1: Parting horizontal element
 2: Complete horizontal element
Further forms: see page 60
HEIDENHAIN MANUALplus 620, CNC PILOT 640
73
2.3 Units—Recessing
"ICP recess turning" unit
The unit machines the contour described by ICP axially/radially from
"NS to NE". The workpiece is machined by alternate recessing and
roughing movements.
The unit machines the contour described in the FINISHED program
section axially/radially from "NS to NE". Any auxiliary contour defined
in FK will be used.
Unit name: G869_ICP / Cycle: G869 (see page 286)
Contour form
X1, Z1
Starting point of blank: Evaluation only if no blank has been
defined
RI, RK
Workpiece blank oversize in X and Z direction
SX, SZ Cutting limit (SX: diameter value)—(default: no cutting limit)
Further parameters of the contour form: see page 62
Cycle form
P
Maximum infeed during rough turning
I, K
Oversize in X, Z direction (I: diameter value)
RB
Turning depth compensation for finishing
B
Offset width
U
Cutting direction
Q
 0 (Bi): Bidirectional (in both directions)
 1 (Uni): Unidirectional (in direction of contour)
Sequence (roughing/finishing)
A
W
O
E
H
 0: Roughing and finishing
 1: Only roughing
 2: Only finishing
Approach angle (default: opposite to recessing direction)
Departure angle (default: opposite to recessing direction)
Recessing feed rate (default: active feed rate)
Finishing feed rate (default: active feed rate)
Type of retraction at end of cycle
 0: Return to starting point
 Axial recess: First Z, then X direction
 Radial recess: First X, then Z direction
 1: Positions in front of the finished contour
 2: Retracts to safety clearance and stops
Further forms: see page 60
The Steuerung uses the tool definition to distinguish between radial
and axial recessing.
Turning depth compensation RB: Depending on factors such as
workpiece material or feed rate, the tool tip is displaced during a
turning operation. You can correct the resulting infeed error with the
turning depth compensation factor. The value is usually determined
empirically.
74
Access to the technology database:
 Machining operation: Recess turning
 Affected parameters: F, S, O, P
smart.Turn units
2.3 Units—Recessing
Offset width B: After the second infeed movement, during the
transition from turning to recessing, the path to be machined is
reduced by "offset width B." Each time the system switches on this
side, the path is reduced by B—in addition to the previous offset. The
total offset is limited to 80 % of the effective cutting width (effective
cutting width = cutting width –2*cutting radius). If required, the
Steuerung reduces the programmed offset width. After clearance
roughing, the remaining material is removed with a single cut.
"Contour recessing with direct contour input"
unit
The unit machines the contour defined by the parameters axially/
radially.
Unit name: G860_G80 / Cycle: G860 (see page 283)
Contour form:
RI, RK
Workpiece blank oversize in X and Z direction
Further parameters of the contour form: see page 62
Cycle form
Q
Roughing/finishing (process variants)
 0: Roughing and finishing
 1: Only roughing
 2: Only finishing
I, K
Oversize in X, Z direction (I: diameter value)
ET
Recessing depth
P
Recessing width (default: 0.8 x tool width)
E
Finishing feed rate: Differing feed rate used only for the
finishing process
EZ
Period of dwell after recessing path (default: time for one
spindle revolution)
D
Revolutions on recessing floor
DQ
Number of recessing cycles
DX, DZ Distance to subsequent recess in X, Z direction
Further forms: see page 60
The Steuerung uses the tool definition to distinguish between radial
and axial recessing.
Access to the technology database:
 Machining operation: Contour recessing
 Affected parameters: F, S, E
HEIDENHAIN MANUALplus 620, CNC PILOT 640
75
2.3 Units—Recessing
"Recess turning with direct contour input" unit
The unit machines the contour defined by the parameters axially/
radially. The workpiece is machined by alternate recessing and
roughing movements. The machining process requires a minimum of
retraction and infeed movements.
Unit name: G869_G80 / Cycle: G869 (see page 286)
Contour form:
RI, RK
Workpiece blank oversize in X and Z direction
Further parameters of the contour form: see page 62
Cycle form
P
Maximum infeed during rough turning
I, K
Oversize in X, Z direction (I: diameter value)
RB
Turning depth compensation for finishing
B
Offset width
U
Cutting direction
Q
 0 (Bi): Bidirectional (in both directions)
 1 (Uni): Unidirectional (in direction of contour)
Sequence (roughing/finishing)
 0: Roughing and finishing
 1: Only roughing
 2: Only finishing
Further forms: see page 60
The Steuerung uses the tool definition to distinguish between radial
and axial recessing.
Turning depth compensation RB: Depending on factors such as
workpiece material or feed rate, the tool tip is displaced during a
turning operation. You can correct the resulting infeed error with the
turning depth compensation factor. The value is usually determined
empirically.
Offset width B: After the second infeed movement, during the
transition from turning to recessing, the path to be machined is
reduced by "offset width B." Each time the system switches on this
side, the path is reduced by B—in addition to the previous offset. The
total offset is limited to 80 % of the effective cutting width (effective
cutting width = cutting width –2*cutting radius). If required, the
Steuerung reduces the programmed offset width. After clearance
roughing, the remaining material is removed with a single cut.
Access to the technology database:
 Machining operation: Recess turning
 Affected parameters: F, S, O, P
76
smart.Turn units
2.3 Units—Recessing
"Parting" unit
The unit parts the workpiece. If programmed, a chamfer or rounding
arc is machined on the outside diameter. At the end of cycle, the tool
returns to the starting point. You can define a feed rate reduction,
which becomes effective as soon as the position I is reached.
Unit name: G859_CUT_OFF / Cycle: G859 (see page 315)
Cycle form
X1, Z1
Starting point of contour in X, Z (X: diameter value)
B
Chamfer/rounding
 B>0: Radius of rounding arc
 B<0: Section length of chamfer
D
Maximum speed
XE
Inside diameter (pipe)
I
Diameter for feed-rate reduction. Limit diameter over
which traverse is at reduced feed rate.
E
Reduced feed rate
SD
Speed limitation from the diameter I up
U
Diameter from which the part catcher is activated
(machine-dependent function)
K
Retraction distance after parting: Lift off the tool laterally
from the plane surface before retraction
Further forms: see page 60
The limit to the maximum speed "D" is only effective in the
cycle. After the cycle ends, the speed limit before the
cycle become effective.
Access to the technology database:
 Machining operation: Contour recessing
 Affected parameters: F, S, E
HEIDENHAIN MANUALplus 620, CNC PILOT 640
77
2.3 Units—Recessing
"Undercutting (H, K, U)" unit
Depending on KG, the unit machines one of the following undercuts:
 Type U: The unit machines an undercut and finishes the adjoining
plane surface. Either a chamfer or a rounding arc can be machined.
 Type H: The end point of the undercut is determined from the
plunging angle.
 Type K: Only one linear cut at an angle of 45° is performed. The
resulting contour geometry therefore depends on the tool that is
used.
 First, you select the Type of undercut KG, and then you
enter the values for the selected type of undercut.
 The Steuerung changes parameters with the same
address letters for the other undercuts as well. Do not
change these values.
Unit name: G85x_H_K_U / Cycle: G85 (see page 316)
Contour form
KG
Type of undercut
 Type U: Cycle G856 (see page 321)
 Type H: Cycle G857 (see page 322)
 Type K: Cycle G858 (see page 323)
X1, Z1
Contour corner point (X: diameter value)
Undercut type U
X2
End point, face (diameter value)
I
Undercut diameter
K
Undercut length
B
Chamfer/rounding
 B>0: Radius of rounding arc
 B<0: Section length of chamfer
Undercut type H
K
Undercut length
R
Radius in the undercut corner
W
Plunge angle
Undercut type K
I
Undercut depth (radius)
Further forms: see page 60
Access to the technology database:
 Machining operation: Finishing
 Affected parameters: F, S
78
smart.Turn units
2.3 Units—Recessing
"ICP recessing" unit
G870 generates a recess defined by G22-Geo. The Steuerung uses
the tool definition to distinguish between external and internal
machining, or between radial and axial recesses.
Unit name: G870_ICP / Cycle: G870 (see page 289)
Contour form
I
Oversize in X and Z direction
EZ
Period of dwell after recessing path (default: time for one
spindle revolution)
Further parameters of the contour form: see page 62
Further forms: see page 60
Access to the technology database:
 Machining operation: Recessing
 Affected parameters: F, S
HEIDENHAIN MANUALplus 620, CNC PILOT 640
79
2.4 Units—Centric drilling
2.4 Units—Centric drilling
"Centric drilling" unit
The unit uses stationary tools to drill axial holes in several passes.
Suitable tools can be positioned up to +/– 2 mm outside the turning
center.
Unit name: G74_ZENTR / Cycle: G74 (see page 331)
Cycle form
Z1
Start point drill (starting point of hole)
Z2
End point drill (end point of hole)
NS
Starting block no. of contour
X
Start point drill (starting point of hole; diameter value)—
(range: –2 mm < X < 2 mm; default: 0)
E
Delay (dwell time at end of hole) (default: 0)
D
Retraction at
V
AB
P
IB
JB
B
RI
 0: Rapid traverse
 1: Feed rate
Feed rate reduction
 0: Without reduction
 1: At end of the hole
 2: At start of the hole
 3: At start and end of the hole
Spot drilling / through drilling length (distance for feed rate
reduction)
Hole depth
Hole depth reduction value: Value by which the feed depth
decreases after every advance.
Minimum hole depth: If you have entered a hole depth
reduction value, the hole depth is reduced only to the value
entered in JB.
Retraction distance: Value by which the tool is retracted
after reaching the respective hole depth.
Internal safety clearance: Distance for reapproach inside
the hole (default: safety clearance SCK).
"Global" form
G14
Tool change point
 No axis
 0: Simultaneously
 1: First X, then Z
 2: First Z, then X
 3: Only X
 4: Only Z
 5: Only Y direction
 6: Simultaneous with Y (X, Y and Z axes move on a
diagonal path)
80
Access to the technology database:
 Machining operation: Drilling
 Affected parameters: F, S
smart.Turn units
Coolant
SCK
 0: Without
 1: Circuit 1 on
 2: Circuit 2 on
Safety clearance in infeed direction: Safety clearance in
infeed direction during drilling and milling operations.
Protection zone. During drilling and boring the protection
zone monitoring is
G60
2.4 Units—Centric drilling
CLT
 0: Active
 1: Inactive
BP
Break duration: Time span for interruption of the feed for
chip breaking.
BF
Feed duration: Time interval until the next break. The
interruption of the feed rate breaks the chip.
Further forms: see page 60
If X is not programmed or XS is in the range of –2 mm < XS
< 2 mm, then the control drills at XS.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
81
2.4 Units—Centric drilling
"Centric tapping" unit
The unit cuts axial threads using stationary tools.
Unit name: G73_ZENTR / Cycle: G73 (see page 328)
Cycle form
Z1
Start point drill (starting point of hole)
Z2
End point drill (end point of hole)
NS
Starting block no. of contour
X
Start point drill (starting point of hole; diameter value)—
(range: –2 mm < X < 2 mm; default: 0)
F1
Thread pitch
B
Run-in length
L
Retraction length when using floating tap holders (default:
0)
SR
Retraction speed (default: Shaft speed for tapping)
SP
Chip breaking depth
SI
Retraction distance
Further forms: see page 60
Retraction length L: Use this parameter for floating tap holders. The
cycle calculates a new nominal pitch on the basis of the thread depth,
the programmed pitch, and the "retraction length." The nominal pitch
is somewhat smaller than the pitch of the tap. During tapping, the tap
is pulled away from the chuck by the retraction length. With this
method you can achieve higher service life from the taps.
Access to the technology database:
 Machining operation: Tapping
 Affected parameters: S
82
smart.Turn units
2.4 Units—Centric drilling
"Boring, centric countersinking" unit
The unit uses stationary tools to drill axial holes in several passes.
Unit name: G72_ZENTR / Cycle: G72 (see page 327)
Cycle form
NS
Starting block no. of contour
E
Delay (dwell time at end of hole) (default: 0)
D
Retraction at
RB
 0: Rapid traverse
 1: Feed rate
Retraction plane
"Global" form
G14
Tool change point
CLT
SCK
G60
 No axis
 0: Simultaneously
 1: First X, then Z
 2: First Z, then X
 3: Only X
 4: Only Z
 5: Only Y direction
 6: Simultaneous with Y (X, Y and Z axes move on a
diagonal path)
Coolant
 0: Without
 1: Circuit 1 on
 2: Circuit 2 on
Safety clearance in infeed direction: Safety clearance in
infeed direction during drilling and milling operations.
Protection zone. During drilling and boring the protection
zone monitoring is
 0: Active
 1: Inactive
Further forms: see page 60
HEIDENHAIN MANUALplus 620, CNC PILOT 640
83
2.5 Units—Drilling in C axis
2.5 Units—Drilling in C axis
"Single hole, face" unit
This unit machines a hole on the face of the workpiece.
Unit name: G74_Bohr_Stirn_C / Cycle: G74 (see page 331)
Cycle form
Z1
Start point drill (starting point of hole)
Z2
End point drill (end point of hole)
CS
Spindle angle
E
Delay (dwell time at end of hole) (default: 0)
D
Retraction at
V
AB
P
IB
JB
B
RI
 0: Rapid traverse
 1: Feed rate
Feed rate reduction
 0: Without reduction
 1: At end of the hole
 2: At start of the hole
 3: At start and end of the hole
Spot drilling / through drilling length – distance for feed rate
reduction
Hole depth
Hole depth reduction value: Value by which the feed depth
decreases after every advance.
Minimum hole depth: If you have entered a hole depth
reduction value, the hole depth is reduced only to the value
entered in JB.
Retraction distance: Value by which the tool is retracted
after reaching the respective hole depth.
Internal safety clearance: Distance for reapproach inside
the hole (default: safety clearance SCK).
Access to the technology database:
 Machining operation: Drilling
 Affected parameters: F, S
"Global" form
G14
Tool change point
 No axis
 0: Simultaneously
 1: First X, then Z
 2: First Z, then X
 3: Only X
 4: Only Z
 5: Only Y direction
 6: Simultaneous with Y (X, Y and Z axes move on a
diagonal path)
84
smart.Turn units
Coolant
SCK
 0: Without
 1: Circuit 1 on
 2: Circuit 2 on
Safety clearance in infeed direction: Safety clearance in
infeed direction during drilling and milling operations.
Protection zone. During drilling and boring the protection
zone monitoring is
G60
2.5 Units—Drilling in C axis
CLT
 0: Active
 1: Inactive
BP
Break duration: Time span for interruption of the feed for
chip breaking.
BF
Feed duration: Time interval until the next break. The
interruption of the feed rate breaks the chip.
Further forms: see page 60
HEIDENHAIN MANUALplus 620, CNC PILOT 640
85
2.5 Units—Drilling in C axis
"Linear pattern drilling, face" unit
The unit machines a linear drilling pattern in which the individual
features are arranged at a regular spacing on the face.
Unit name: G74_Lin_Stirn_C / Cycle: G74 (see page 331)
Pattern form
Q
Number of holes
X1, C1 Polar starting point
XK, YK Cartesian starting point
I, J
End point (XK, YK)
Ii, Ji:
Distance (XKi, YKi)
R
Distance to first/last hole
Ri
Incremental distance
A
Pattern angle (reference is XK axis)
Cycle form
Z1
Start point drill (starting point of hole)
Z2
End point drill (end point of hole)
E
Delay (dwell time at end of hole) (default: 0)
D
Retraction at
V
AB
P
IB
JB
B
RI
RB
86
 0: Rapid traverse
 1: Feed rate
Feed rate reduction
 0: Without reduction
 1: At end of the hole
 2: At start of the hole
 3: At start and end of the hole
Spot drilling / through drilling length (distance for feed rate
reduction)
Hole depth
Hole depth reduction value: Value by which the feed depth
decreases after every advance.
Minimum hole depth: If you have entered a hole depth
reduction value, the hole depth is reduced only to the value
entered in JB.
Retraction distance: Value by which the tool is retracted
after reaching the respective hole depth.
Internal safety clearance: Distance for reapproach inside
the hole (default: safety clearance SCK).
Retraction plane (default: return to the starting position or
to the safety clearance)
Access to the technology database:
 Machining operation: Drilling
 Affected parameters: F, S
smart.Turn units
2.5 Units—Drilling in C axis
"Global" form
G14
Tool change point
CLT
SCK
G60
 No axis
 0: Simultaneously
 1: First X, then Z
 2: First Z, then X
 3: Only X
 4: Only Z
 5: Only Y direction
 6: Simultaneous with Y (X, Y and Z axes move on a
diagonal path)
Coolant
 0: Without
 1: Circuit 1 on
 2: Circuit 2 on
Safety clearance in infeed direction: Safety clearance in
infeed direction during drilling and milling operations.
Protection zone. During drilling and boring the protection
zone monitoring is
 0: Active
 1: Inactive
BP
Break duration: Time span for interruption of the feed for
chip breaking.
BF
Feed duration: Time interval until the next break. The
interruption of the feed rate breaks the chip.
Further forms: see page 60
HEIDENHAIN MANUALplus 620, CNC PILOT 640
87
2.5 Units—Drilling in C axis
"Circular pattern drilling, face" unit
This unit machines a circular drilling pattern on the face of the
workpiece.
Unit name: G74_Cir_Stirn_C / Cycle: G74 (see page 331)
Pattern form
Q
Number of holes
XM, CM Polar center point
XK, YK
Cartesian center point
A
Starting angle
Wi
Angle increment
K
Pattern diameter
W
End angle
VD
Rotation direction (default: 0)
 VD=0, without W: Figures are arranged on a full circle
 VD=0, with W: Figures are arranged on the longer
circular arc
 VD=0, with Wi: The algebraic sign of Wi defines the
direction (Wi<0: clockwise)
 VD=1, with W: Clockwise
 VD=1, with Wi: Clockwise (algebraic sign of Wi has no
effect)
 VD=2, with W: Counterclockwise
 VD=2, with Wi: Counterclockwise (algebraic sign of Wi
has no effect)
Cycle form
Z1
Start point drill (starting point of hole)
Z2
End point drill (end point of hole)
E
Delay (dwell time at end of hole) (default: 0)
D
Retraction at
V
AB
P
IB
JB
B
88
 0: Rapid traverse
 1: Feed rate
Feed rate reduction
 0: Without reduction
 1: At end of the hole
 2: At start of the hole
 3: At start and end of the hole
Spot drilling / through drilling length (distance for feed rate
reduction)
First hole depth
Hole depth reduction value: Value by which the feed depth
decreases after every advance.
Minimum hole depth: If you have entered a hole depth
reduction value, the hole depth is reduced only to the
value entered in JB.
Retraction distance: Value by which the tool is retracted
after reaching the respective hole depth.
Access to the technology database:
 Machining operation: Drilling
 Affected parameters: F, S
smart.Turn units
2.5 Units—Drilling in C axis
RI
Internal safety clearance: Distance for reapproach inside
the hole (default: safety clearance SCK).
RB
Retraction plane (default: return to the starting position or
to the safety clearance)
Further forms: see page 60
"Global" form
G14
Tool change point
CLT
SCK
G60
 No axis
 0: Simultaneously
 1: First X, then Z
 2: First Z, then X
 3: Only X
 4: Only Z
 5: Only Y direction
 6: Simultaneous with Y (X, Y and Z axes move on a
diagonal path)
Coolant
 0: Without
 1: Circuit 1 on
 2: Circuit 2 on
Safety clearance in infeed direction: Safety clearance in
infeed direction during drilling and milling operations.
Protection zone. During drilling and boring the protection
zone monitoring is
 0: Active
 1: Inactive
BP
Break duration: Time span for interruption of the feed for
chip breaking.
BF
Feed duration: Time interval until the next break. The
interruption of the feed rate breaks the chip.
Further forms: see page 60
HEIDENHAIN MANUALplus 620, CNC PILOT 640
89
2.5 Units—Drilling in C axis
"Tapping, face" unit
This unit machines a single tap hole on the face of the workpiece.
Unit name: G73_Gew_Stirn_C / Cycle: G73 (see page 328)
Cycle form
Z1
Start point drill (starting point of hole)
Z2
End point drill (end point of hole)
CS
Spindle angle
F1
Thread pitch
B
Run-in length
L
Retraction length when using floating tap holders (default: 0)
SR
Retraction speed (default: Shaft speed for tapping)
SP
Chip breaking depth
SI
Retraction distance
Further forms: see page 60
Use the retraction length for floating tap holders. The cycle
calculates a new nominal pitch on the basis of the thread depth, the
programmed pitch, and the retraction length. The nominal pitch is
somewhat smaller than the pitch of the tap. During tapping, the tap is
pulled away from the chuck by the retraction length. With this method
you can achieve higher service life from taps.
Access to the technology database:
 Machining operation: Tapping
 Affected parameters: S
90
smart.Turn units
2.5 Units—Drilling in C axis
"Linear tapping pattern, face" unit
The unit machines a linear tapping pattern in which the individual
features are arranged at a regular spacing on the face.
Unit name: G73_Lin_Stirn_C / Cycle: G73 (see page 328)
Pattern form
Q
Number of holes
X1, C1 Polar starting point
XK, YK Cartesian starting point
I, J
End point (XK, YK)
Ii, Ji:
Distance (XKi, YKi)
R
Distance to first/last hole
Ri
Incremental distance
A
Pattern angle (reference is XK axis)
Cycle form
Z1
Start point drill (starting point of hole)
Z2
End point drill (end point of hole)
F1
Thread pitch
B
Run-in length
L
Retraction length when using floating tap holders (default: 0)
SR
Retraction speed (default: Shaft speed for tapping)
SP
Chip breaking depth
SI
Retraction distance
RB
Retraction plane (default: return to the starting position or
to the safety clearance)
Further forms: see page 60
Use the retraction length for floating tap holders. The cycle
calculates a new nominal pitch on the basis of the thread depth, the
programmed pitch, and the retraction length. The nominal pitch is
somewhat smaller than the pitch of the tap. During tapping, the tap is
pulled away from the chuck by the retraction length. With this method
you can achieve higher service life from taps.
Access to the technology database:
 Machining operation: Tapping
 Affected parameters: S
HEIDENHAIN MANUALplus 620, CNC PILOT 640
91
2.5 Units—Drilling in C axis
"Circular tapping pattern, face" unit
This unit machines a circular tapping pattern on the face of the
workpiece.
Unit name: G73_Cir_Stirn_C / Cycle: G73 (see page 328)
Pattern form
Q
Number of holes
XM, CM Polar center point
XK, YK
Cartesian center point
A
Starting angle
Wi
Angle increment
K
Pattern diameter
W
End angle
VD
Rotation direction (default: 0)
 VD=0, without W: Figures are arranged on a full circle
 VD=0, with W: Figures are arranged on the longer
circular arc
 VD=0, with Wi: The algebraic sign of Wi defines the
direction (Wi<0: clockwise)
 VD=1, with W: Clockwise
 VD=1, with Wi: Clockwise (algebraic sign of Wi has no
effect)
 VD=2, with W: Counterclockwise
 VD=2, with Wi: Counterclockwise (algebraic sign of Wi
has no effect)
Cycle form
Z1
Start point drill (starting point of hole)
Z2
End point drill (end point of hole)
F1
Thread pitch
B
Run-in length
L
Retraction length when using floating tap holders (default:
0)
SR
Retraction speed (default: Shaft speed for tapping)
SP
Chip breaking depth
SI
Retraction distance
RB
Retraction plane (default: return to the starting position or
to the safety clearance)
Further forms: see page 60
Use the retraction length for floating tap holders. The cycle
calculates a new nominal pitch on the basis of the thread depth, the
programmed pitch, and the retraction length. The nominal pitch is
somewhat smaller than the pitch of the tap. During tapping, the tap is
pulled away from the chuck by the retraction length. With this method
you can achieve higher service life from taps.
Access to the technology database:
 Machining operation: Tapping
 Affected parameters: S
92
smart.Turn units
2.5 Units—Drilling in C axis
"Single hole, lateral surface" unit
This unit machines a hole on the lateral surface of the workpiece.
Unit name: G74_Bohr_Mant_C / Cycle: G74 (see page 331)
Cycle form
X1
Start point drill (starting point of hole; diameter value)
X2
End point drill (end point of hole; diameter value)
CS
Spindle angle
E
Delay (dwell time at end of hole) (default: 0)
D
Retraction at
V
AB
P
IB
JB
B
RI
 0: Rapid traverse
 1: Feed rate
Feed rate reduction
 0: Without reduction
 1: At end of the hole
 2: At start of the hole
 3: At start and end of the hole
Spot drilling / through drilling length (distance for feed rate
reduction)
Hole depth
Hole depth reduction value: Value by which the feed depth
decreases after every advance.
Minimum hole depth: If you have entered a hole depth
reduction value, the hole depth is reduced only to the value
entered in JB.
Retraction distance: Value by which the tool is retracted
after reaching the respective hole depth.
Internal safety clearance: Distance for reapproach inside
the hole (default: safety clearance SCK).
"Global" form
G14
Tool change point
CLT
 No axis
 0: Simultaneously
 1: First X, then Z
 2: First Z, then X
 3: Only X
 4: Only Z
 5: Only Y direction
 6: Simultaneous with Y (X, Y and Z axes move on a
diagonal path)
Coolant
Access to the technology database:
 Machining operation: Drilling
 Affected parameters: F, S
 0: Without
 1: Circuit 1 on
 2: Circuit 2 on
HEIDENHAIN MANUALplus 620, CNC PILOT 640
93
2.5 Units—Drilling in C axis
SCK
Safety clearance in infeed direction: Safety clearance in
infeed direction during drilling and milling operations.
BP
Break duration: Time span for interruption of the feed for
chip breaking.
BF
Feed duration: Time interval until the next break. The
interruption of the feed rate breaks the chip.
Further forms: see page 60
94
smart.Turn units
2.5 Units—Drilling in C axis
"Linear pattern drilling, lateral surface" unit
The unit machines a linear drilling pattern in which the individual
features are arranged at a regular spacing on the lateral surface.
Unit name: G74_Lin_Mant_C / Cycle: G74 (see page 331)
Pattern form
Q
Number of holes
Z1, C1
Starting point of pattern
Wi
Angle increment
W
End angle
Z2
End point of pattern
Cycle form
X1
Start point drill (starting point of hole; diameter value)
X2
End point drill (end point of hole; diameter value)
E
Delay (dwell time at end of hole) (default: 0)
D
Retraction at
V
AB
P
IB
JB
B
RI
RB
 0: Rapid traverse
 1: Feed rate
Feed rate reduction
 0: Without reduction
 1: At end of the hole
 2: At start of the hole
 3: At start and end of the hole
Spot drilling / through drilling length (distance for feed rate
reduction)
Hole depth
Hole depth reduction value: Value by which the feed depth
decreases after every advance.
Minimum hole depth: If you have entered a hole depth
reduction value, the hole depth is reduced only to the value
entered in JB.
Retraction distance: Value by which the tool is retracted
after reaching the respective hole depth.
Internal safety clearance: Distance for reapproach inside
the hole (default: safety clearance SCK).
Retraction plane (default: return to the starting position or
to the safety clearance)
Access to the technology database:
 Machining operation: Drilling
 Affected parameters: F, S
HEIDENHAIN MANUALplus 620, CNC PILOT 640
95
2.5 Units—Drilling in C axis
"Global" form
G14
Tool change point
CLT
 No axis
 0: Simultaneously
 1: First X, then Z
 2: First Z, then X
 3: Only X
 4: Only Z
 5: Only Y direction
 6: Simultaneous with Y (X, Y and Z axes move on a
diagonal path)
Coolant
 0: Without
 1: Circuit 1 on
 2: Circuit 2 on
SCK
Safety clearance in infeed direction: Safety clearance in
infeed direction during drilling and milling operations.
BP
Break duration: Time span for interruption of the feed for
chip breaking.
BF
Feed duration: Time interval until the next break. The
interruption of the feed rate breaks the chip.
Further forms: see page 60
96
smart.Turn units
2.5 Units—Drilling in C axis
"Circular pattern drilling, lateral surface" unit
This unit machines a circular hole pattern on the lateral surface of the
workpiece.
Unit name: G74_Cir_Mant_C / Cycle: G74 (see page 331)
Pattern form
Q
Number of holes
ZM, CM Center point of pattern
A
Starting angle
Wi
Angle increment
K
Pattern diameter
W
End angle
VD
Rotation direction (default: 0)
 VD=0, without W: Figures are arranged on a full circle
 VD=0, with W: Figures are arranged on the longer
circular arc
 VD=0, with Wi: The algebraic sign of Wi defines the
direction (Wi<0: clockwise)
 VD=1, with W: Clockwise
 VD=1, with Wi: Clockwise (algebraic sign of Wi has no
effect)
 VD=2, with W: Counterclockwise
 VD=2, with Wi: Counterclockwise (algebraic sign of Wi
has no effect)
Cycle form
X1
Start point drill (starting point of hole; diameter value)
X2
End point drill (end point of hole; diameter value)
E
Delay (dwell time at end of hole) (default: 0)
D
Retraction at:
V
AB
P
IB
JB
B
 0: Rapid traverse
 1: Feed rate
Feed rate reduction:
 0: Without reduction
 1: At end of the hole
 2: At start of the hole
 3: At start and end of the hole
Spot drilling / through drilling length (distance for feed rate
reduction)
Hole depth
Hole depth reduction value: Value by which the feed depth
decreases after every advance.
Minimum hole depth: If you have entered a hole depth
reduction value, the hole depth is reduced only to the
value entered in JB.
Retraction distance: Value by which the tool is retracted
after reaching the respective hole depth.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
Access to the technology database:
 Machining operation: Drilling
 Affected parameters: F, S
97
2.5 Units—Drilling in C axis
RI
RB
Internal safety clearance: Distance for reapproach inside
the hole (default: safety clearance SCK).
Retraction plane (default: return to the starting position or
to the safety clearance)
"Global" form
G14
Tool change point
CLT
 No axis
 0: Simultaneously
 1: First X, then Z
 2: First Z, then X
 3: Only X
 4: Only Z
 5: Only Y direction
 6: Simultaneous with Y (X, Y and Z axes move on a
diagonal path)
Coolant
 0: Without
 1: Circuit 1 on
 2: Circuit 2 on
SCK
Safety clearance in infeed direction: Safety clearance in
infeed direction during drilling and milling operations.
BP
Break duration: Time span for interruption of the feed for
chip breaking.
BF
Feed duration: Time interval until the next break. The
interruption of the feed rate breaks the chip.
Further forms: see page 60
98
smart.Turn units
2.5 Units—Drilling in C axis
"Tap hole, lateral surface" unit
This unit machines a tap hole on the lateral surface of the workpiece.
Unit name: G73_Gew_Mant_C / Cycle: G73 (see page 328)
Cycle form
X1
Start point drill (starting point of hole; diameter value)
X2
End point drill (end point of hole; diameter value)
CS
Spindle angle
F1
Thread pitch
B
Run-in length
L
Retraction length when using floating tap holders (default: 0)
SR
Retraction speed (default: Shaft speed for tapping)
SP
Chip breaking depth
SI
Retraction distance
Further forms: see page 60
Use the retraction length for floating tap holders. The cycle
calculates a new nominal pitch on the basis of the thread depth, the
programmed pitch, and the retraction length. The nominal pitch is
somewhat smaller than the pitch of the tap. During tapping, the tap is
pulled away from the chuck by the retraction length. With this method
you can achieve higher service life from taps.
Access to the technology database:
 Machining operation: Tapping
 Affected parameters: S
HEIDENHAIN MANUALplus 620, CNC PILOT 640
99
2.5 Units—Drilling in C axis
"Linear tapping pattern, lateral surface" unit
The unit machines a linear tapping pattern in which the individual
features are arranged at a regular spacing on the lateral surface.
Unit name: G73_Lin_Mant_C / Cycle: G73 (see page 328)
Pattern form
Q
Number of holes
Z1, C1
Starting point of pattern
Wi
Angle increment
W
End angle
Z2
End point of pattern
Cycle form
X1
Start point drill (starting point of hole; diameter value)
X2
End point drill (end point of hole; diameter value)
F1
Thread pitch
B
Run-in length
L
Retraction length when using floating tap holders (default: 0)
SR
Retraction speed (default: Shaft speed for tapping)
SP
Chip breaking depth
SI
Retraction distance
RB
Retraction plane
Further forms: see page 60
Use the retraction length for floating tap holders. The cycle
calculates a new nominal pitch on the basis of the thread depth, the
programmed pitch, and the retraction length. The nominal pitch is
somewhat smaller than the pitch of the tap. During tapping, the tap is
pulled away from the chuck by the retraction length. With this method
you can achieve higher service life from taps.
Access to the technology database:
 Machining operation: Tapping
 Affected parameters: S
100
smart.Turn units
2.5 Units—Drilling in C axis
"Circular tapping pattern, lateral surface" unit
This unit machines a circular tapping pattern on the lateral surface of
the workpiece.
Unit name: G73_Cir_Mant_C / Cycle: G73 (see page 328)
Pattern form
Q
Number of holes
ZM, CM Center point of pattern
A
Starting angle
Wi
Angle increment
K
Pattern diameter
W
End angle
VD
Rotation direction (default: 0)
 VD=0, without W: Figures are arranged on a full circle
 VD=0, with W: Figures are arranged on the longer
circular arc
 VD=0, with Wi: The algebraic sign of Wi defines the
direction (Wi<0: clockwise)
 VD=1, with W: Clockwise
 VD=1, with Wi: Clockwise (algebraic sign of Wi has no
effect)
 VD=2, with W: Counterclockwise
 VD=2, with Wi: Counterclockwise (algebraic sign of Wi
has no effect)
Cycle form
X1
Start point drill (starting point of hole; diameter value)
X2
End point drill (end point of hole; diameter value)
F1
Thread pitch
B
Run-in length
L
Retraction length when using floating tap holders (default: 0)
SR
Retraction speed (default: Shaft speed for tapping)
SP
Chip breaking depth
SI
Retraction distance
RB
Retraction plane
Further forms: see page 60
Access to the technology database:
 Machining operation: Tapping
 Affected parameters: S
Use the retraction length for floating tap holders. The cycle
calculates a new nominal pitch on the basis of the thread depth, the
programmed pitch, and the retraction length. The nominal pitch is
somewhat smaller than the pitch of the tap. During tapping, the tap is
pulled away from the chuck by the retraction length. With this method
you can achieve higher service life from taps.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
101
2.5 Units—Drilling in C axis
"ICP drilling, C axis" unit
The unit machines a single hole or a hole pattern on the face or lateral
surface. Using ICP, you define the holes as well as further details.
Unit name: G74_ICP_C / Cycle: G74 (see page 331)
Pattern form
FK
Finished part contour
NS
Starting block no. of contour
Cycle form
E
Delay (dwell time at end of hole) (default: 0)
D
Retraction at
V
AB
P
IB
JB
B
RI
RB
102
 0: Rapid traverse
 1: Feed rate
Feed rate reduction
 0: Without reduction
 1: At end of the hole
 2: At start of the hole
 3: At start and end of the hole
Spot drilling / through drilling length (distance for feed rate
reduction)
Hole depth
Hole depth reduction value: Value by which the feed depth
decreases after every advance.
Minimum hole depth: If you have entered a hole depth
reduction value, the hole depth is reduced only to the value
entered in JB.
Retraction distance: Value by which the tool is retracted
after reaching the respective hole depth.
Internal safety clearance: Distance for reapproach inside
the hole (default: safety clearance SCK).
Retraction plane (default: return to the starting position or
to the safety clearance)
Access to the technology database:
 Machining operation: Drilling
 Affected parameters: F, S
smart.Turn units
2.5 Units—Drilling in C axis
"Global" form
G14
Tool change point
CLT
 No axis
 0: Simultaneously
 1: First X, then Z
 2: First Z, then X
 3: Only X
 4: Only Z
 5: Only Y direction
 6: Simultaneous with Y (X, Y and Z axes move on a
diagonal path)
Coolant
 0: Without
 1: Circuit 1 on
 2: Circuit 2 on
SCK
Safety clearance in infeed direction: Safety clearance in
infeed direction during drilling and milling operations.
BP
Break duration: Time span for interruption of the feed for
chip breaking.
BF
Feed duration: Time interval until the next break. The
interruption of the feed rate breaks the chip.
Further forms: see page 60
HEIDENHAIN MANUALplus 620, CNC PILOT 640
103
2.5 Units—Drilling in C axis
"ICP tapping, C axis" unit
The unit machines a single tap hole or a tapping pattern on the face or
lateral surface. Using ICP, you define the tap holes as well as further
details.
Unit name: G73_ICP_C / Cycle: G73 (see page 328)
Pattern form
FK
see page 62
NS
Starting block no. of contour
Cycle form
F1
Thread pitch
B
Run-in length
L
Retraction length when using floating tap holders (default: 0)
SR
Retraction speed (default: Shaft speed for tapping)
SP
Chip breaking depth
SI
Retraction distance
RB
Retraction plane
Further forms: see page 60
Use the retraction length for floating tap holders. The cycle
calculates a new nominal pitch on the basis of the thread depth, the
programmed pitch, and the retraction length. The nominal pitch is
somewhat smaller than the pitch of the tap. During tapping, the tap is
pulled away from the chuck by the retraction length. With this method
you can achieve higher service life from taps.
104
Access to the technology database:
 Machining operation: Tapping
 Affected parameters: S
smart.Turn units
2.5 Units—Drilling in C axis
"ICP boring/countersinking, C axis" unit
The unit machines a single hole or a hole pattern on the face or lateral
surface. Using ICP, you define the hole positions as well as further
details for boring or countersinking.
Unit name: G72_ICP_C / Cycle: G72 (see page 327)
Pattern form
FK
see page 62
NS
Starting block no. of contour
Cycle form
E
Delay (dwell time at end of hole) (default: 0)
D
Retraction at
 0: Rapid traverse
 1: Feed rate
RB
Retraction plane (default: return to the starting position or
to the safety clearance)
Further forms: see page 60
Access to the technology database:
 Machining operation: Drilling
 Affected parameters: F, S
HEIDENHAIN MANUALplus 620, CNC PILOT 640
105
2.6 Units—Predrilling in C axis
2.6 Units—Predrilling in C axis
"Predrill, contour mill, figures on face" unit
The unit determines the hole position and machines the hole. The
subsequent milling cycle obtains the hole position from the reference
stored in NF.
Unit name: DRILL_STI_KON_C / Cycles: G840 A1 (see page 359); G71
(see page 325)
Figure form
Q
Type of figure
QN
X1
C1
Z1
P2
L
 0: Full circle
 1: Linear slot
 2: Circular slot
 3: Triangle
 4: Rectangle, square
 5: Polygon
Number of polygon corners—only with Q=5 (polygon)
Diameter of figure center
Angle of figure center
Milling top edge
Depth of figure
Edge length / width across flats
B
RE
A
Q2
 L>0: Edge length
 L<0: Width across flats (inside diameter) for polygon
Rectangle width
Rounding radius
Angle to X axis
Rotational direction of slot—only if Q=2 (circular slot)
W
 cw: In clockwise direction
 ccw: In counterclockwise direction
Angle of slot end point—only if Q=2 (circular slot)
Program only the parameters relevant to the selected
figure type.
Access to the technology database:
 Machining operation: Drilling
 Affected parameters: F, S
106
smart.Turn units
2.6 Units—Predrilling in C axis
Cycle form
JK
Cutter position
H
 0: On the contour
 1: Within the contour
 2: Outside the contour
Cutting direction
I
K
R
WB
NF
E
D
 0: Up-cut milling
 1: Climb milling
Contour-parallel oversize
Infeed-direction oversize
Approach radius
Cutter diameter
Position mark
Delay (dwell time at end of hole) (default: 0)
Retraction at
V
 0: Rapid traverse
 1: Feed rate
Feed rate reduction
 0: Without reduction
 1: At end of the hole
 2: At start of the hole
 3: At start and end of the hole
AB
Spot drilling / through drilling length (distance for feed rate
reduction)
RB
Retraction plane (default: return to the starting position or
to the safety clearance)
Further forms: see page 60
HEIDENHAIN MANUALplus 620, CNC PILOT 640
107
2.6 Units—Predrilling in C axis
"Predrill, contour mill, ICP on face" unit
The unit determines the hole position and machines the hole. The
subsequent milling cycle obtains the hole position from the reference
stored in NF. If the milling contour consists of multiple sections, the
unit machines a hole for each section.
Unit name: DRILL_STI_840_C / Cycles: G840 A1 (see page 359); G71
(see page 325)
Contour form
FK
see page 62
NS
Starting block no. of contour
NE
End block no. of contour
Z1
Milling top edge
P2
Depth of contour
Cycle form
JK
Cutter position
H
 0: On the contour
 1, closed contour: Within the contour
 1, open contour: Left of the contour
 2, closed contour: Outside the contour
 2, open contour: Right of the contour
 3: Depending on H and MD
Cutting direction
I
K
R
WB
NF
E
D
 0: Up-cut milling
 1: Climb milling
Contour-parallel oversize
Infeed-direction oversize
Approach radius
Cutter diameter
Position mark
Delay (dwell time at end of hole) (default: 0)
Retraction at
V
 0: Rapid traverse
 1: Feed rate
Feed rate reduction
 0: Without reduction
 1: At end of the hole
 2: At start of the hole
 3: At start and end of the hole
AB
Spot drilling / through drilling length (distance for feed rate
reduction)
RB
Retraction plane (default: return to the starting position or
to the safety clearance)
Further forms: see page 60
108
Access to the technology database:
 Machining operation: Drilling
 Affected parameters: F, S
smart.Turn units
2.6 Units—Predrilling in C axis
"Predrill, pocket mill, figures on face" unit
The unit determines the hole position and machines the hole. The
subsequent milling cycle obtains the hole position from the reference
stored in NF.
Unit name: DRILL_STI_TASC / Cycles: G845 A1 (see page 369); G71
(see page 325)
Figure form
Q
Type of figure
QN
X1
C1
Z1
P2
L
 0: Full circle
 1: Linear slot
 2: Circular slot
 3: Triangle
 4: Rectangle, square
 5: Polygon
Number of polygon corners—only with Q=5 (polygon)
Diameter of figure center
Angle of figure center
Milling top edge
Depth of figure
Edge length / width across flats
B
RE
A
Q2
 L>0: Edge length
 L<0: Width across flats (inside diameter) for polygon
Rectangle width
Rounding radius
Angle to X axis
Rotational direction of slot—only if Q=2 (circular slot)
W
 cw: In clockwise direction
 ccw: In counterclockwise direction
Angle of slot end point—only if Q=2 (circular slot)
Program only the parameters relevant to the selected
figure type.
Access to the technology database:
 Machining operation: Drilling
 Affected parameters: F, S
HEIDENHAIN MANUALplus 620, CNC PILOT 640
109
2.6 Units—Predrilling in C axis
Cycle form
JT
Machining direction
H
 0: From the inside out (from the inside towards the
outside)
 1: From the outside in (from the outside towards the
inside)
Cutting direction
I
K
U
WB
NF
E
D
 0: Up-cut milling
 1: Climb milling
Contour-parallel oversize
Infeed-direction oversize
Overlap factor (default: 0.5)
Cutter diameter
Position mark
Delay (dwell time at end of hole) (default: 0)
Retraction at
V
 0: Rapid traverse
 1: Feed rate
Feed rate reduction
 0: Without reduction
 1: At end of the hole
 2: At start of the hole
 3: At start and end of the hole
AB
Spot drilling / through drilling length (distance for feed rate
reduction)
RB
Retraction plane (default: return to the starting position or
to the safety clearance)
Further forms: see page 60
110
smart.Turn units
2.6 Units—Predrilling in C axis
"Predrill, pocket mill, ICP on face" unit
The unit determines the hole position and machines the hole. The
subsequent milling cycle obtains the hole position from the reference
stored in NF. If the pocket consists of multiple sections, the unit
machines a hole for each section.
Unit name: DRILL_STI_845_C / Cycles: G845 A1 (see page 369); G71
(see page 325)
Contour form
FK
see page 62
NS
Starting block no. of contour
NE
End block no. of contour
Z1
Milling top edge
P2
Depth of contour
Cycle form
JT
Machining direction
H
 0: From the inside out (from the inside towards the
outside)
 1: From the outside in (from the outside towards the
inside)
Cutting direction
I
K
U
WB
NF
E
D
 0: Up-cut milling
 1: Climb milling
Contour-parallel oversize
Infeed-direction oversize
Overlap factor (default: 0.5)
Cutter diameter
Position mark
Delay (dwell time at end of hole) (default: 0)
Retraction at
V
 0: Rapid traverse
 1: Feed rate
Feed rate reduction
 0: Without reduction
 1: At end of the hole
 2: At start of the hole
 3: At start and end of the hole
AB
Spot drilling / through drilling length (distance for feed rate
reduction)
RB
Retraction plane (default: return to the starting position or
to the safety clearance)
Further forms: see page 60
Access to the technology database:
 Machining operation: Drilling
 Affected parameters: F, S
HEIDENHAIN MANUALplus 620, CNC PILOT 640
111
2.6 Units—Predrilling in C axis
"Predrill, contour mill, figures on lateral surface"
unit
The unit determines the hole position and machines the hole. The
subsequent milling cycle obtains the hole position from the reference
stored in NF.
Unit name: DRILL_MAN_KON_C / Cycles: G840 A1 (see page 359);
G71 (see page 325)
Figure form
Q
Type of figure
QN
Z1
C1
CY
X1
P2
L
 0: Full circle
 1: Linear slot
 2: Circular slot
 3: Triangle
 4: Rectangle, square
 5: Polygon
Number of polygon corners—only with Q=5 (polygon)
Figure center
Angle of figure center
Figure center of unrolled lateral surface
Milling top edge
Depth of figure
Edge length / width across flats
B
RE
A
Q2
 L>0: Edge length
 L<0: Width across flats (inside diameter) for polygon
Rectangle width
Rounding radius
Angle to Z axis
Rotational direction of slot—only if Q=2 (circular slot)
W
 cw: In clockwise direction
 ccw: In counterclockwise direction
Angle of slot end point—only if Q=2 (circular slot)
Program only the parameters relevant to the selected
figure type.
Access to the technology database:
 Machining operation: Drilling
 Affected parameters: F, S
112
smart.Turn units
2.6 Units—Predrilling in C axis
Cycle form
JK
Cutter position
H
 0: On the contour
 1: Within the contour
 2: Outside the contour
Cutting direction
I
K
R
WB
NF
E
D
 0: Up-cut milling
 1: Climb milling
Contour-parallel oversize
Infeed-direction oversize
Approach radius
Cutter diameter
Position mark
Delay (dwell time at end of hole) (default: 0)
Retraction at
V
 0: Rapid traverse
 1: Feed rate
Feed rate reduction
 0: Without reduction
 1: At end of the hole
 2: At start of the hole
 3: At start and end of the hole
AB
Spot drilling / through drilling length (distance for feed rate
reduction)
RB
Retraction plane (default: return to the starting position or
to the safety clearance)
Further forms: see page 60
HEIDENHAIN MANUALplus 620, CNC PILOT 640
113
2.6 Units—Predrilling in C axis
"Predrill, contour mill, ICP on lateral surface"
unit
The unit determines the hole position and machines the hole. The
subsequent milling cycle obtains the hole position from the reference
stored in NF. If the milling contour consists of multiple sections, the
unit machines a hole for each section.
Unit name: DRILL_MAN_840_C / Cycles: G840 A1 (see page 359);
G71 (see page 325)
Contour form
FK
see page 62
NS
Starting block no. of contour
NE
End block no. of contour
X1
Milling top edge (diameter value)
P2
Depth of contour (radius value)
Cycle form
JK
Cutter position
H
 0: On the contour
 1, closed contour: Within the contour
 1, open contour: Left of the contour
 2, closed contour: Outside the contour
 2, open contour: Right of the contour
 3: Depending on H and MD
Cutting direction
I
K
R
WB
NF
E
D
 0: Up-cut milling
 1: Climb milling
Contour-parallel oversize
Infeed-direction oversize
Approach radius
Cutter diameter
Position mark
Delay (dwell time at end of hole) (default: 0)
Retraction at
V
 0: Rapid traverse
 1: Feed rate
Feed rate reduction
 0: Without reduction
 1: At end of the hole
 2: At start of the hole
 3: At start and end of the hole
AB
Spot drilling / through drilling length (distance for feed rate
reduction)
RB
Retraction plane (diameter value)
Further forms: see page 60
114
Access to the technology database:
 Machining operation: Drilling
 Affected parameters: F, S
smart.Turn units
2.6 Units—Predrilling in C axis
"Predrill, pocket mill, figures on lateral surface"
unit
The unit determines the hole position and machines the hole. The
subsequent milling cycle obtains the hole position from the reference
stored in NF.
Unit name: DRILL_MAN_TAS_C / Cycles: G845 A1 (see page 369);
G71 (see page 325)
Figure form
Q
Type of figure
QN
Z1
C1
CY
X1
P2
L
 0: Full circle
 1: Linear slot
 2: Circular slot
 3: Triangle
 4: Rectangle, square
 5: Polygon
Number of polygon corners—only with Q=5 (polygon)
Figure center
Angle of figure center
Figure center of unrolled lateral surface
Milling top edge
Depth of figure
Edge length / width across flats
B
RE
A
Q2
 L>0: Edge length
 L<0: Width across flats (inside diameter) for polygon
Rectangle width
Rounding radius
Angle to Z axis
Rotational direction of slot—only if Q=2 (circular slot)
W
 cw: In clockwise direction
 ccw: In counterclockwise direction
Angle of slot end point—only if Q=2 (circular slot)
Program only the parameters relevant to the selected
figure type.
Access to the technology database:
 Machining operation: Drilling
 Affected parameters: F, S
HEIDENHAIN MANUALplus 620, CNC PILOT 640
115
2.6 Units—Predrilling in C axis
Cycle form
JT
Machining direction
H
 0: From the inside out (from the inside towards the
outside)
 1: From the outside in (from the outside towards the
inside)
Cutting direction
I
K
U
WB
NF
E
D
 0: Up-cut milling
 1: Climb milling
Infeed-direction oversize
Contour-parallel oversize
Overlap factor (default: 0.5)
Cutter diameter
Position mark
Delay (dwell time at end of hole) (default: 0)
Retraction at
V
 0: Rapid traverse
 1: Feed rate
Feed rate reduction
 0: Without reduction
 1: At end of the hole
 2: At start of the hole
 3: At start and end of the hole
AB
Spot drilling / through drilling length (distance for feed rate
reduction)
RB
Retraction plane (default: return to the starting position or
to the safety clearance)
Further forms: see page 60
116
smart.Turn units
2.6 Units—Predrilling in C axis
"Predrill, pocket mill, ICP on lateral surface" unit
The unit determines the hole position and machines the hole. The
subsequent milling cycle obtains the hole position from the reference
stored in NF. If the pocket consists of multiple sections, the unit
machines a hole for each section.
Unit name: DRILL_MAN_845_C / Cycles: G845 A1 (see page 369);
G71 (see page 325)
Contour form
FK
see page 62
NS
Starting block no. of contour
NE
End block no. of contour
X1
Milling top edge (diameter value)
P2
Depth of contour
Cycle form
JT
Machining direction
H
 0: From the inside out (from the inside towards the
outside)
 1: From the outside in (from the outside towards the
inside)
Cutting direction
I
K
U
WB
NF
E
D
 0: Up-cut milling
 1: Climb milling
Infeed-direction oversize
Contour-parallel oversize
Overlap factor (default: 0.5)
Cutter diameter
Position mark
Delay (dwell time at end of hole) (default: 0)
Retraction at
V
 0: Rapid traverse
 1: Feed rate
Feed rate reduction
 0: Without reduction
 1: At end of the hole
 2: At start of the hole
 3: At start and end of the hole
AB
Spot drilling / through drilling length (distance for feed rate
reduction)
RB
Retraction plane (diameter value)
Further forms: see page 60
Access to the technology database:
 Machining operation: Drilling
 Affected parameters: F, S
HEIDENHAIN MANUALplus 620, CNC PILOT 640
117
2.7 Units—Finishing
2.7 Units—Finishing
"ICP contour finishing" unit
The unit finishes the contour described by ICP from "NS to NE" in one
pass.
Unit name: G890_ICP / Cycle: G890 (see page 290)
Contour form
B
Switch on TRC (type of tool radius compensation)
HR
 0: Automatic
 1: Tool to the left (G41)
 2: Tool to the right (G42)
 3: Automatic, without tool angle compensation
 4: Tool to the left (G41), without tool angle compensation
 5: Tool to the right (G42), without tool angle
compensation
Main cutting direction
 0: Automatic
 1: +Z
 2: +X
 3: -Z
 4: -X
SX, SZ Cutting limit (SX: diameter value)—(default: no cutting limit)
Further parameters of the contour form: see page 62
Cycle form
Q
Type of approach (default: 0)
 0: Automatic selection—the Steuerung checks:
 Diagonal approach
 First X, then Z direction
 Equidistant around the barrier
 Omission of the first contour elements if the starting
position is inaccessible
 1: First X, then Z direction
 2: First Z, then X direction
 3: No approach—tool is located near the starting point of
the contour area.
Access to the technology database:
 Machining operation: Finishing
 Affected parameters: F, S
118
smart.Turn units
2.7 Units—Finishing
Cycle form
H
Type of retraction. Tool backs off at 45° against the
machining direction and moves to the position I, K (default:
3):
D
E
 0: Diagonal
 1: First X, then Z direction
 2: First Z, then X direction
 3: Stops at safety clearance
 4: No retraction motion (tool remains on the end
coordinate)
 5: Diagonal to start position
 6: First X, then Z direction to start position
 7: First Z, then X direction to start position
 8: With G1 to I and K
Cycle end position. Position that is approached at the end
of the cycle (I: diameter value).
Omit elements (see figure)
Plunging behavior
O
 E=0: Descending contours are not machined
 E>0: Plunging feed rate for declining contour elements.
Descending contour elements are machined.
 No input: The plunging feed rate is reduced during
machining of declining contour elements by up to 50 %.
Descending contour elements are machined.
Feed rate reduction for circular elements (default: 0)
I, K
 0: Feed rate reduction is active
 1: No feed rate reduction
DXX
Additive correction numbers 1 – 16
G58
Contour-parallel oversize (radius)
DI
Axis-parallel oversize X
DK
Axis-parallel oversize Z
Further forms: see page 60
If feed rate reduction is active, at least four spindle
revolutions are used to machine every "small" contour
element.
With the address Dxx you activate an additive
compensation for the entire cycle run. The additive
compensation is switched off again at the end of the cycle.
You edit additive compensation values in the Program Run
mode of operation.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
119
2.7 Units—Finishing
"Longitudinal finishing with direct contour
input" unit
The unit finishes the contour defined by the parameters in one pass.
In EC you define whether you want to machine a normal or a plunging
contour.
Unit name: G890_G80_L / Cycle: G890 (see page 290)
Contour form
EC
Type of contour
 0: Normal contour
 1: Plunging contour
X1, Z1
Contour starting point
X2, Z2
Contour end point
RC
Rounding: Radius of contour corner
AC
Start angle: Angle of the first contour element
(range: 0° < AC < 90°)
WC
End angle: Angle of the last contour element
(range: 0° < WC < 90°)
BS
Chamfer/radius at start
 BS>0: Radius of rounding arc
 BS<0: Section length of chamfer
BE
Chamfer/radius at end
 BE>0: Radius of rounding arc
 BE<0: Section length of chamfer
Cycle form
E
Plunging behavior
 E>0: Plunging feed rate for declining contour elements.
Descending contour elements are machined.
 No input: The plunging feed rate is reduced during
machining of declining contour elements by up to 50 %.
Descending contour elements are machined.
B
Switch on TRC (type of tool radius compensation)
 0: Automatic
 1: Tool to the left (G41)
 2: Tool to the right (G42)
 3: Automatic, without tool angle compensation
 4: Tool to the left (G41), without tool angle compensation
 5: Tool to the right (G42), without tool angle
compensation
DXX
Additive correction numbers 1 – 16
G58
Contour-parallel oversize (radius)
Further forms: see page 60
With the address Dxx you activate an additive
compensation for the entire cycle run. The additive
compensation is switched off again at the end of the cycle.
You edit additive compensation values in the Program Run
mode of operation.
120
Access to the technology database:
 Machining operation: Finishing
 Affected parameters: F, S, E
smart.Turn units
2.7 Units—Finishing
"Transverse finishing with direct contour input"
unit
The unit finishes the contour defined by the parameters in one pass.
In EC you define whether you want to machine a normal or a plunging
contour.
Unit name: G890_G80_P / Cycle: G890 (see page 290)
Contour form
EC
Type of contour
 0: Normal contour
 1: Plunging contour
X1, Z1
Contour starting point
X2, Z2
Contour end point
RC
Rounding: Radius of contour corner
AC
Start angle: Angle of the first contour element
(range: 0° < AC < 90°)
WC
End angle: Angle of the last contour element
(range: 0° < WC < 90°)
BS
Chamfer/radius at start:
 BS>0: Radius of rounding arc
 BS<0: Section length of chamfer
BE
Chamfer/radius at end
 BE>0: Radius of rounding arc
 BE<0: Section length of chamfer
Cycle form
E
Plunging behavior
 E>0: Plunging feed rate for declining contour elements.
Descending contour elements are machined.
 No input: The plunging feed rate is reduced during
machining of declining contour elements by up to 50 %.
Descending contour elements are machined.
B
Switch on TRC (type of tool radius compensation)
 0: Automatic
 1: Tool to the left (G41)
 2: Tool to the right (G42)
 3: Automatic, without tool angle compensation
 4: Tool to the left (G41), without tool angle compensation
 5: Tool to the right (G42), without tool angle
compensation
DXX
Additive correction numbers 1 – 16
G58
Contour-parallel oversize (radius)
Further forms: see page 60
With the address Dxx you activate an additive
compensation for the entire cycle run. The additive
compensation is switched off again at the end of the cycle.
You edit additive compensation values in the Program Run
mode of operation.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
Access to the technology database:
 Machining operation: Finishing
 Affected parameters: F, S, E
121
2.7 Units—Finishing
"Relief turns (undercut) type E, F, DIN76" unit
The unit machines the undercut defined by KG, and then the adjoining
plane surface. The cylinder chamfer is executed when you enter at
least one of the parameters 1st cut length or 1st cut radius.
Unit name: G85x_DIN_E_F_G / Cycle: G85 (see page 316)
Overview form
KG
Type of relief turn (undercut)
 E: DIN 509 type E; Cycle G851 (see page 318)
 F: DIN 509 type F; Cycle G852 (see page 319)
 G: DIN 76 type G (thread undercut); Cycle G853 (see
page 320)
X1, Z1
Contour starting point (X1: diameter value)
X2, Z2
Contour end point (X2: diameter value)
App
Approach see page 65
Parameters on the "Type E" form
I
Undercut depth (default: value from standard table)
K
Undercut length (default: value from standard table)
W
Undercut angle (default: 15° from standard table)
R
Undercut radius (default: value from standard table)
H
Type of departure
 0: To the starting point
 1: Plane surface end
Parameters on the "Type F" form
I
Undercut depth (default: value from standard table)
K
Undercut length (default: value from standard table)
W
Undercut angle (default: 15° from standard table)
R
Undercut radius (default: value from standard table)
P2
Face depth (default: value from standard table)
A
Face angle (default: 8° from standard table)
H
Type of departure
 0: To the starting point
 1: Plane surface end
Access to the technology database:
 Machining operation: Finishing
 Affected parameters: F, S, E
122
smart.Turn units
2.7 Units—Finishing
Parameters on the "Type G" form
FP
Thread pitch
I
Undercut diameter (default: value from standard table)
K
Undercut length (default: value from standard table)
W
Undercut angle (default: 30° from standard table)
R
Undercut radius (default: value from standard table)
P1
Undercut oversize
H
 No input: Machining in one cut
 P1>0: Division into pre-turning and finish-turning; P1 is
the longitudinal oversize; the transverse oversize is
always 0.1 mm
Type of departure
 0: To the starting point
 1: Plane surface end
Additional parameters for "cylinder first cut"
B
Cylinder 1st cut length (no input: no cylinder start chamfer)
WB
1st cut angle (default: 45°)
RB
Positive value: 1st cut radius, negative value: chamfer (no
input: no element)
E
Reduced feed rate for plunging and the first cut (default:
active feed rate)
U
Grinding oversize for cylinder
Further forms: see page 60
Access to the technology database:
 Machining operation: Finishing
 Affected parameters: F, S, E
 Undercuts can only be executed in orthogonal, paraxial
contour corners along the longitudinal axis.
 Parameters that are not programmed are automatically
calculated by the Steuerung from the standard table.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
123
2.7 Units—Finishing
"Measuring cut" unit
The unit performs a cylindrical measuring cut with the length defined
in the cycle, moves to the breakpoint for measuring and stops the
program. After the program was stopped, you can manually measure
the workpiece.
Unit name: MEASURE_G809 / Cycle: G809 (see page 293)
Contour form
EC
Machining location
 0: Outside
 1: Inside
XA, ZA Contour starting point
R
Measuring cut length
P
Measuring cut oversize
O
Approach angle: If an approach angle is entered, the cycle
positions the tool over the starting point taking into account
the safety clearance, and from there plunges at the
specified angle to the diameter to be measured.
ZR
Workpiece blank starting point: Collision-free approach for
inside machining
Cycle form
QC
Machining direction
V
D
WE
 0: -Z
 1: +Z
Measuring cut counter: Number of workpieces after which
a measurement is performed
Additive correction numbers 1 – 16
Directions
 0: Simultaneously
 1: First X, then Z
 2: First Z, then X
Xi, Zi:
Additive correction numbers 1 – 16
AX
Departing position X
Further forms: see page 60
124
smart.Turn units
2.8 Units—Threads
2.8 Units—Threads
Overview of thread units
 "Thread, direct" cuts a simple internal or external thread in
longitudinal direction.
 "ICP thread" cuts a single or multi-start internal or external thread
in longitudinal or transverse direction. The contour on which the
thread is cut is defined with ICP.
 "API thread" cuts a single or multi-start API thread. The depth of
thread decreases at the overrun at the end of thread.
 "Tapered thread" cuts a single or multi-start tapered internal or
external thread.
Handwheel superimposition
If your machine features handwheel superimposition, you can overlap
axis movements during thread cutting in a limited area:
 X direction: Maximum programmed thread depth depending on the
current cutting depth
 Z direction: +/- a fourth of the thread pitch
Machine and control must be specially prepared by the
machine tool builder for use of this cycle. Refer to your
machine manual.
Remember that position changes resulting from
handwheel superimposition are no longer effective after
the cycle end or the "last cut" function.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
125
2.8 Units—Threads
Parameter V: Type of infeed
With the V parameter you define the type of infeed for thread cutting
cycles.
The following infeed types are available:
0: Constant mach. X-section
The control reduces the cutting depth after each infeed to
achieve a consistent chip cross section and removal rate.
1: Constant infeed
The control uses the same cutting depth for each infeed without
exceeding the maximum infeed I.
2: EPL with distribution of cuts
The control uses the thread pitch F1 and the constant shaft speed
S to calculate the cutting depth for a constant infeed. If the thread
depth is not a multiple of the cutting depth, the control uses the
depth of the remaining cut for the first infeed. With the
"distribution of remaining cuts," the control divides the last cutting
depth into four partial cuts. The first cut is half the calculated
cutting depth, the second is a quarter and the third and fourth
each are an eighth.
3: EPL without distribution of cuts
The control uses the thread pitch F1 and the constant shaft speed
S to calculate the cutting depth for a constant infeed. If the thread
depth is not a multiple of the cutting depth, the control uses the
depth of the remaining cut for the first infeed. All subsequent
infeeds are constant and correspond to the calculated cutting
depth.
4: MANUALplus 4110
The control performs the first infeed with the maximum infeed I.
To determine the subsequent cutting depths, the control uses
the formula gt = 2 * I * SQRT "current no. of cuts", where "gt" is
the absolute depth. The cutting depth decreases with each
infeed since the current number of cuts is incremented by 1 with
each infeed. If, as a result, the remaining cut depth R falls below
the value defined in R, the control uses the value from R as the
new constant cutting depth! If the thread depth is not a multiple
of the cutting depth, the control performs the last cut to the final
depth.
5: Constant infeed (4290)
The control uses the same cutting depth for each infeed; the
cutting depth corresponds to the maximum infeed I. If the thread
depth is not a multiple of the cutting depth, the control uses the
depth of the remaining cut for the first infeed.
126
smart.Turn units
2.8 Units—Threads
6: Constant infeed with remaining cutting (4290)
The control uses the same cutting depth for each infeed; the
cutting depth corresponds to the maximum infeed I. If the thread
depth is not a multiple of the cutting depth, the control uses the
depth of the remaining cut for the first infeed. With the
"distribution of remaining cuts," the control divides the last cutting
depth into four partial cuts. The first cut is half the calculated
cutting depth, the second is a quarter and the third and fourth
each are an eighth.
"Thread, direct" unit
The unit cuts a simple internal or external thread in longitudinal
direction.
Unit name: G32_MAN / Cycle: G32 (see page 307)
Thread form
O
Thread location
KE
 0: Internal thread (infeed in +X)
 1: External thread (infeed in –X)
Approach see page 65
Start diameter
Starting position Z
End point of thread
Thread pitch
Thread depth (automatically for metric ISO threads)
Maximum infeed (radius)
Number of cuts (only if I is not programmed and the infeed
V is 0 or 1)
Run-out position
K
 0: At the end of the threading cut
 1: At the start of the threading cut
Run-out length
APP
XS
ZS
Z2
F1
U
I
IC
Access to the technology database:
 Machining operation: Thread cutting
 Affected parameters: F, S
HEIDENHAIN MANUALplus 620, CNC PILOT 640
127
2.8 Units—Threads
Cycle form
H
Kind of displacement (type of offset; offset between the
individual infeeds in cutting direction)
V
 0: Without offset
 1: From left
 2: From right
 3: Alternately left/right
Type of infeed (for details, see page 126)
 0: Constant mach. X-section
 1: Constant infeed
 2: W/ remaining cutting (with distribution of remaining
cuts)
 3: W/o remaining cutting (without distribution of
remaining cuts)
 4: Same as MANUALplus 4110
 5: Constant infeed (same as 4290)
 6: Constant with distribute. (same as 4290)
A
Approach angle (angle of infeed; reference: X axis;
0°<A<60°; default: 30°)
R
Remaining cut depth (only with V=4)
C
Starting angle
D
No. of gears (threads per unit)
Q
No. no load (number of dry runs)
Further forms: see page 60
"ICP thread" unit
The unit cuts a single or multi-start internal or external thread in
longitudinal or transverse direction. The contour on which the thread
is cut is defined with ICP.
Unit name: G31_ICP / Cycle: G31 (see page 303)
Thread form
FK
Auxiliary contour: see page 62
NS
Starting block no. of contour
NE
End block no. of contour
O1
Machine form element
O
 0: No machining
 1: At beginning
 2: At end
 3: At beginning and end
 4: Only chamfer and rounding arc
Thread location
Access to the technology database:
 Machining operation: Thread cutting
 Affected parameters: F, S
 0: Internal thread (infeed in +X)
 1: External thread (infeed in –X)
128
smart.Turn units
2.8 Units—Threads
J1
Thread orientation
 From 1st contour element
 0: Longitudinal
 1: Transverse
F1
Thread pitch
U
Thread depth (automatically for metric ISO threads)
A
Approach angle (angle of infeed; reference: X axis; 60°<A<60°; default: 30°)
D
No. of gears (threads per unit)
K
Run-out length
Cycle form
H
Kind of displacement (type of offset; offset between the
individual infeeds in cutting direction)
V
 0: Without offset
 1: From left
 2: From right
 3: Alternately left/right
Type of infeed (for details, see page 126)
 0: Constant mach. X-section
 1: Constant infeed
 2: W/ remaining cutting (with distribution of remaining
cuts)
 3: W/o remaining cutting (without distribution of
remaining cuts)
 4: Same as MANUALplus 4110
 5: Constant infeed (same as 4290)
 6: Constant with distribute. (same as 4290)
R
Remaining cut depth (only with V=4)
I
Maximum infeed (radius)
IC
Number of cuts (only if I is not programmed)
B
Run-in length
P
Overrun length
C
Starting angle
Q
No. no load (number of dry runs)
Further forms: see page 60
HEIDENHAIN MANUALplus 620, CNC PILOT 640
129
2.8 Units—Threads
"API thread" unit
This unit cuts a single or multi-start API thread. The depth of thread
decreases at the overrun at the end of thread.
Unit name: G352_API / Cycle: G352 (see page 312)
Thread form
O
Thread location
 0: Internal thread (infeed in +X)
 1: External thread (infeed in –X)
X1, Z1
Starting point of thread (X1: diameter value)
X2, Z2
End point of thread (X2: diameter value)
W
Taper angle (reference: Z axis; –45°<W<45°)
WE
Run-out angle (reference: Z axis; 0°<WE<90°; default: 12°)
F1
Thread pitch
U
Thread depth (automatically for metric ISO threads)
Cycle form
I
Maximum infeed (radius)
H
Kind of displacement (type of offset; offset between the
individual infeeds in cutting direction)
V
 0: Without offset
 1: From left
 2: From right
 3: Alternately left/right
Type of infeed (for details, see page 126)
 0: Constant mach. X-section
 1: Constant infeed
 2: W/ remaining cutting (with distribution of remaining
cuts)
 3: W/o remaining cutting (without distribution of
remaining cuts)
 4: Same as MANUALplus 4110
 5: Constant infeed (same as 4290)
 6: Constant with distribute. (same as 4290)
A
Approach angle (angle of infeed; reference: X axis; 60°<A<60°; default: 30°)
R
Remaining cut depth (only with V=4)
C
Starting angle
D
No. of gears (threads per unit)
Q
No. no load (number of dry runs)
Further forms: see page 60
Access to the technology database:
 Machining operation: Thread cutting
 Affected parameters: F, S
130
smart.Turn units
2.8 Units—Threads
"Tapered thread" unit
The unit cuts a single or multi-start tapered internal or external thread.
Unit name: G32_KEG / Cycle: G32 (see page 307)
Thread form
O
Thread location
X1, Z1
X2, Z2
W
F1
U
KE
 0: Internal thread (infeed in +X)
 1: External thread (infeed in –X)
Starting point of thread (X1: diameter value)
End point of thread (X2: diameter value)
Taper angle (reference: Z axis; –45°<W<45°)
Thread pitch
Thread depth (automatically for metric ISO threads)
Run-out position
K
 0: At the end of the threading cut
 1: At the start of the threading cut
Run-out length
Access to the technology database:
 Machining operation: Thread cutting
 Affected parameters: F, S
HEIDENHAIN MANUALplus 620, CNC PILOT 640
131
2.8 Units—Threads
Cycle form
I
Maximum infeed (radius)
IC
Number of cuts (only if I is not programmed)
H
Kind of displacement (type of offset; offset between the
individual infeeds in cutting direction)
V
 0: Without offset
 1: From left
 2: From right
 3: Alternately left/right
Type of infeed (for details, see page 126)
 0: Constant mach. X-section
 1: Constant infeed
 2: W/ remaining cutting (with distribution of remaining
cuts)
 3: W/o remaining cutting (without distribution of
remaining cuts)
 4: Same as MANUALplus 4110
 5: Constant infeed (same as 4290)
 6: Constant with distribute. (same as 4290)
A
Approach angle (angle of infeed; reference: X axis;
0°<A<60°; default: 30°)
R
Remaining cut depth (only with V=4)
C
Starting angle
D
No. of gears (threads per unit)
Q
No. no load (number of dry runs)
Further forms: see page 60
132
smart.Turn units
2.9 Units—Milling, face
2.9 Units—Milling, face
"Slot, face" unit
The unit mills a slot from the starting position to the end point on the
face of the workpiece. The slot width equals the diameter of the
milling cutter.
Unit name: G791_Nut_Stirn_C / Cycle: G791 (see page 349)
Cycle form
Z1
Milling top edge
Z2
Milling floor
L
Slot length
A1
Angle to X axis
X1, C1 Polar slot target point
XK, YK Cartesian slot target point
P
Maximum infeed
FZ
Infeed rate
Further forms: see page 60
Access to the technology database:
 Machining operation: Milling
 Affected parameters: F, S, FZ, P
HEIDENHAIN MANUALplus 620, CNC PILOT 640
133
2.9 Units—Milling, face
"Linear slot pattern, face" unit
The unit machines a linear slot pattern in which the individual features
are arranged at a regular spacing on the face of the workpiece. The
starting points of the slots correspond to the pattern positions. You
define the length and the position of the slots in the unit. The slot
width equals the diameter of the milling cutter.
Unit name: G791_Lin_Stirn_C / Cycle: G791 (see page 349)
Pattern form
Q
Number of slots
X1, C1 Polar starting point
XK, YK Cartesian starting point
I, J
End point (XK, YK)
Ii, Ji:
Distance (XKi, YKi)
R
Distance to first/last contour
Ri
Incremental distance
A
Pattern angle (reference is XK axis)
Cycle form
Z1
Milling top edge
Z2
Milling floor
L
Slot length
A1
Angle to X axis
P
Maximum infeed
FZ
Infeed rate
Further forms: see page 60
Access to the technology database:
 Machining operation: Milling
 Affected parameters: F, S, FZ, P
134
smart.Turn units
2.9 Units—Milling, face
"Circular slot pattern, face" unit
The unit machines a circular slot pattern in which the individual
features are arranged at a regular spacing on the face of the
workpiece. The starting points of the slots correspond to the pattern
positions. You define the length and the position of the slots in the
unit. The slot width equals the diameter of the milling cutter.
Unit name: G791_Cir_Stirn_C / Cycle: G791 (see page 349)
Pattern form
Q
Number of slots
XM, CM Polar center point
XK, YK
Cartesian center point
A
Starting angle
Wi
Angle increment
K
Pattern diameter
W
End angle
V
Rotation direction (default: 0)
 VD=0, without W: Figures are arranged on a full circle
 VD=0, with W: Figures are arranged on the longer
circular arc
 VD=0, with Wi: The algebraic sign of Wi defines the
direction (Wi<0: clockwise)
 VD=1, with W: Clockwise
 VD=1, with Wi: Clockwise (algebraic sign of Wi has no
effect)
 VD=2, with W: Counterclockwise
 VD=2, with Wi: Counterclockwise (algebraic sign of Wi
has no effect)
Cycle form
Z1
Milling top edge
Z2
Milling floor
L
Slot length
A1
Angle to X axis
P
Maximum infeed
FZ
Infeed rate
Further forms: see page 60
Access to the technology database:
 Machining operation: Milling
 Affected parameters: F, S, FZ, P
HEIDENHAIN MANUALplus 620, CNC PILOT 640
135
2.9 Units—Milling, face
"Face milling" unit
Depending on Q, the unit mills surfaces or the defined figure. The unit
cuts the material around the figures.
Unit name: G797_Stirnfr_C / Cycle: G797 (see page 355)
Figure form
Q
Type of figure
 0: Full circle
 1: Single surface
 2: Width across flats
 3: Triangle
 4: Rectangle, square
 5: Polygon
QN
Number of polygon corners (only with Q=5 polygon)
X1
Diameter of figure center
C1
Angle of figure center
Z1
Milling top edge
Z2
Milling floor
X2
Limit diameter
L
Edge length
B
Width/Width across flats
RE
Rounding radius
A
Angle to X axis
Cycle form
QK
Machining operation
J
 Roughing
 Finishing
Milling direction
H
 0: Unidirectional
 1: Bidirectional
Cutting direction
 0: Up-cut milling
 1: Climb milling
P
Maximum infeed
I
Contour-parallel oversize
K
Infeed-direction oversize
FZ
Infeed rate
E
Reduced feed rate
U
Overlap factor
Further forms: see page 60
136
Access to the technology database:
 Machining operation: Finish milling
 Affected parameters: F, S, FZ, P
smart.Turn units
2.9 Units—Milling, face
"Face milling ICP" unit
The unit mills the contour defined with ICP on the face of the
workpiece.
Unit name: G797_ICP / Cycle: G797 (see page 355)
Contour form
FK
see page 62
NS
Starting block no. of contour
Z1
Milling top edge
Z2
Milling floor
X2
Limit diameter
Cycle form
QK
Machining operation
J
 Roughing
 Finishing
Milling direction
H
 0: Unidirectional
 1: Bidirectional
Cutting direction
 0: Up-cut milling
 1: Climb milling
P
Maximum infeed
I
Contour-parallel oversize
K
Infeed-direction oversize
FZ
Infeed rate
E
Reduced feed rate
U
Overlap factor
Further forms: see page 60
HEIDENHAIN MANUALplus 620, CNC PILOT 640
Access to the technology database:
 Machining operation: Finish milling
 Affected parameters: F, S, FZ, P
137
2.9 Units—Milling, face
"Thread milling" unit
The unit mills a thread in existing holes.
Place the tool on the center of the hole before calling G799. The cycle
positions the tool on the end point of the thread within the hole. Then
the tool approaches on "approach radius R" and mills the thread. During
this, the tool advances by the thread pitch F. Following that, the cycle
retracts the tool and returns it to the starting point. With parameter V,
you can program whether the thread is to be milled in one rotation or,
with single-point tools, in several rotations.
Unit name: G799_Gewindefr_C / Cycle: G799 (see page 338)
Position form
Z1
Start point drill (starting point of hole)
P2
Thread depth
I
Thread diameter
F1
Thread pitch
Cycle form
J
Direction of thread
H
 0: Right-hand thread
 1: Left-hand thread
Cutting direction
V
 0: Up-cut milling
 1: Climb milling
Milling method
 0: The thread is milled in a 360-degree helix
 1: The thread is milled in several helical paths (singlepoint tool)
R
Approach radius
Further forms: see page 60
138
Access to the technology database:
 Machining operation: Finish milling
 Affected parameters: F, S
smart.Turn units
2.9 Units—Milling, face
"Contour milling, figures, face" unit
The unit mills the contour defined by Q on the face of the workpiece.
Unit name: G840_Fig_Stirn_C/ Cycle: G840 (see page 361)
Figure form
Q
Type of figure
QN
X1
C1
Z1
P2
L
 0: Full circle
 1: Linear slot
 2: Circular slot
 3: Triangle
 4: Rectangle, square
 5: Polygon
Number of polygon corners—only with Q=5 (polygon)
Diameter of figure center
Angle of figure center
Milling top edge
Depth of figure
Edge length / width across flats
B
RE
A
Q2
 L>0: Edge length
 L<0: Width across flats (inside diameter) for polygon
Rectangle width
Rounding radius
Angle to X axis
Rotational direction of slot—only if Q=2 (circular slot)
W
 cw: In clockwise direction
 ccw: In counterclockwise direction
Angle of slot end point—only if Q=2 (circular slot)
Program only the parameters relevant to the selected
figure type.
Access to the technology database:
 Machining operation: Milling
 Affected parameters: F, S, FZ, P
HEIDENHAIN MANUALplus 620, CNC PILOT 640
139
2.9 Units—Milling, face
Cycle form
JK
Cutter position
H
 0: On the contour
 1: Within the contour
 2: Outside the contour
Cutting direction
P
I
K
FZ
E
R
O
 0: Up-cut milling
 1: Climb milling
Maximum infeed
Contour-parallel oversize
Infeed-direction oversize
Infeed rate
Reduced feed rate
Approach radius
Plunging behavior
NF
 0: Straight (vertical plunge)—The cycle moves the tool to
the starting point; the tool plunges at feed rate and mills
the contour.
 1: In predrilling—The cycle positions the tool above the
hole; the tool plunges and mills the contour.
Position mark (only if O=1)
"Global" form
RB
Retraction plane
Further parameters: see page 64
Further forms: see page 60
140
smart.Turn units
2.9 Units—Milling, face
"ICP contour milling, face" unit
The unit mills the contour defined with ICP on the face of the
workpiece.
Unit name: G840_Kon_C_Stirn / Cycle: G840 (see page 361)
Contour form
FK
see page 62
NS
Starting block no. of contour
NE
End block no. of contour
Z1
Milling top edge
P2
Depth of contour
Cycle form
JK
Cutter position
H
 0: On the contour
 1, closed contour: Within the contour
 1, open contour: Left of the contour
 2, closed contour: Outside the contour
 2, open contour: Right of the contour
 3: Depending on H and MD
Cutting direction
P
I
K
FZ
E
R
O
 0: Up-cut milling
 1: Climb milling
Maximum infeed
Contour-parallel oversize
Infeed-direction oversize
Infeed rate
Reduced feed rate
Approach radius
Plunging behavior
 0: Straight (vertical plunge)—The cycle moves the tool to
the starting point; the tool plunges at feed rate and mills
the contour.
 1: In predrilling—The cycle positions the tool above the
hole; the tool plunges and mills the contour.
NF
Position mark (only if O=1)
RB
Retraction plane
Further forms: see page 60
HEIDENHAIN MANUALplus 620, CNC PILOT 640
141
2.9 Units—Milling, face
"Pocket milling, figures, face" unit
The unit mills the pocket defined by Q. In QK, select the machining
operation (roughing/finishing) and the plunging strategy.
Unit name: G84x_Fig_Stirn_C / Cycles: G845 (see page 370); G846
(see page 374)
Figure form
Q
Type of figure
QN
X1
C1
Z1
P2
L
 0: Full circle
 1: Linear slot
 2: Circular slot
 3: Triangle
 4: Rectangle, square
 5: Polygon
Number of polygon corners—only with Q=5 (polygon)
Diameter of figure center
Angle of figure center
Milling top edge
Depth of figure
Edge length / width across flats
B
RE
A
Q2
 L>0: Edge length
 L<0: Width across flats (inside diameter) for polygon
Rectangle width
Rounding radius
Angle to X axis
Rotational direction of slot—only if Q=2 (circular slot)
W
 cw: In clockwise direction
 ccw: In counterclockwise direction
Angle of slot end point—only if Q=2 (circular slot)
Program only the parameters relevant to the selected
figure type.
Access to the technology database:
 Machining operation: Milling
 Affected parameters: F, S, FZ, P
142
smart.Turn units
2.9 Units—Milling, face
Cycle form
QK
Machining operation and plunging strategy
JT
 0: Roughing
 1: Finishing
 2: Helical roughing, manual
 3: Helical roughing, automatic
 4: Reciprocating linear roughing, manual
 5: Reciprocating linear roughing, automatic
 6: Reciprocating circular roughing, manual
 7: Reciprocating circular roughing, automatic
 8: Plunge roughing at predrilling position
 9: Finishing with 3-D approach arc
Machining direction
H
 0: From the inside out (from the inside towards the
outside)
 1: From the outside in (from the outside towards the
inside)
Cutting direction
P
I
K
FZ
E
R
WB
EW
NF
U
 0: Up-cut milling
 1: Climb milling
Maximum infeed
Contour-parallel oversize
Infeed-direction oversize
Infeed rate
Reduced feed rate
Approach radius
Plunging length
Plunge angle
Position mark (only if QK=8)
Overlap factor (default: 0.5)
"Global" form
RB
Retraction plane
Further parameters: see page 64
Further forms: see page 60
HEIDENHAIN MANUALplus 620, CNC PILOT 640
143
2.9 Units—Milling, face
"ICP pocket milling, face" unit
The unit mills the pocket defined by Q. In QK, select the machining
operation (roughing/finishing) and the plunging strategy.
Unit name: G845_Tas_C_Stirn / Cycles: G845 (see page 370); G846
(see page 374)
Contour form
FK
see page 62
NS
Starting block no. of contour
NE
End block no. of contour
Z1
Milling top edge
P2
Depth of contour
NF
Position mark (only if QK=8)
Cycle form
QK
Machining operation and plunging strategy
JT
 0: Roughing
 1: Finishing
 2: Helical roughing, manual
 3: Helical roughing, automatic
 4: Reciprocating linear roughing, manual
 5: Reciprocating linear roughing, automatic
 6: Reciprocating circular roughing, manual
 7: Reciprocating circular roughing, automatic
 8: Plunge roughing at predrilling position
 9: Finishing with 3-D approach arc
Machining direction
H
 0: From the inside out (from the inside towards the
outside)
 1: From the outside in (from the outside towards the
inside)
Cutting direction
 0: Up-cut milling
 1: Climb milling
P
Maximum infeed
I
Contour-parallel oversize
K
Infeed-direction oversize
FZ
Infeed rate
E
Reduced feed rate
R
Approach radius
WB
Plunging length
EW
Plunge angle
U
Overlap factor (default: 0.5)
RB
Retraction plane
Further forms: see page 60
144
Access to the technology database:
 Machining operation: Milling
 Affected parameters: F, S, FZ, P
smart.Turn units
2.9 Units—Milling, face
"Engraving, face" unit
The unit engraves character strings in linear or polar layout on the face
of the workpiece. Diacritics and special characters that you cannot
enter in the smart.Turn editor can be defined, character by character,
in NF. If you program "Continue from last text" (Q=1), tool change and
pre-positioning are suppressed. The technological data of the previous
engraving cycle apply.
Unit name: G801_GRA_STIRN_C / Cycle: G801 (see page 378)
Character set: see page 376
Position form
X, C
Polar starting point
XK, YK Cartesian starting point
Z
End point. Z position, infeed depth during milling.
RB
Retraction plane
Cycle form
TXT
Text to be engraved
NF
Character number (character to be engraved)
H
Font height
E
Distance factor (for calculation see figure)
W
Inclination angle
FZ
Plunging feed rate factor (plunging feed rate = current feed
rate * FZ)
V
Execution
D
Q
 0: Linear
 1: Arched above
 2: Arched below
Reference diameter
Continue from last text
 0 (No): Engraving starts at the starting point
 1 (Yes): Engraving starts at the tool position
Further forms: see page 60
Access to the technology database:
 Machining operation: Engraving
 Affected parameters: F, S
HEIDENHAIN MANUALplus 620, CNC PILOT 640
145
2.9 Units—Milling, face
"Deburring, face" unit
The unit deburrs the contour defined with ICP on the face of the
workpiece.
Unit name: G840_ENT_C_STIRN / Cycle: G840 (see page 365)
Contour form
FK
see page 62
NS
Starting block no. of contour
NE
End block no. of contour
Z1
Milling top edge
Cycle form
JK
Cutter position
H
 JK=0: On the contour
 JK=1, closed contour: Within the contour
 JK=1, open contour: Left of the contour
 JK=2, closed contour: Outside the contour
 JK=2, open contour: Right of the contour
 JK=3: Depending on H and MD
Cutting direction
 0: Up-cut milling
 1: Climb milling
BG
Chamfer width
JG
Preparation diameter
P
Plunging depth (indicated as a negative value)
I
Contour-parallel oversize
R
Approach radius
FZ
Infeed rate
E
Reduced feed rate
RB
Retraction plane
Further forms: see page 60
Access to the technology database:
 Machining operation: Deburring
 Affected parameters: F, S
146
smart.Turn units
2.10 Units—Milling, lateral surface
2.10 Units—Milling, lateral surface
"Slot, lateral surface" unit
The unit mills a slot from the starting position to the end point on the
lateral surface. The slot width equals the diameter of the milling cutter.
Unit name: G792_Nut_MANT_C / Cycle: G792 (see page 350)
Cycle form
X1
Milling top edge (diameter value)
X2
Milling floor (diameter value)
L
Slot length
A1
Angle to Z axis
Z1, C1
Polar slot target point
P
Maximum infeed
FZ
Infeed rate
Further forms: see page 60
Access to the technology database:
 Machining operation: Milling
 Affected parameters: F, S, FZ, P
HEIDENHAIN MANUALplus 620, CNC PILOT 640
147
2.10 Units—Milling, lateral surface
"Linear slot pattern, lateral surface" unit
The unit machines a linear slot pattern in which the individual features
are arranged at a regular spacing on the lateral surface. The starting
points of the slots correspond to the pattern positions. You define the
length and the position of the slots in the unit. The slot width equals
the diameter of the milling cutter.
Unit name: G792_Lin_Mant_C / Cycle: G792 (see page 350)
Pattern form
Q
Number of slots
Z1, C1
Starting point of pattern
Wi
Angle increment
W
End angle
Z2
End point of pattern
Cycle form
X1
Milling top edge (diameter value)
X2
Milling floor (diameter value)
L
Slot length
A1
Angle to Z axis
P
Maximum infeed
FZ
Infeed rate
Further forms: see page 60
Access to the technology database:
 Machining operation: Milling
 Affected parameters: F, S, FZ, P
148
smart.Turn units
2.10 Units—Milling, lateral surface
"Circular slot pattern, lateral surface" unit
The unit machines a circular slot pattern in which the individual
features are arranged at a regular spacing on the lateral surface. The
starting points of the slots correspond to the pattern positions. You
define the length and the position of the slots in the unit. The slot
width equals the diameter of the milling cutter.
Unit name: G792_Cir_Mant_C / Cycle: G792 (see page 350)
Pattern form
Q
Number of slots
ZM, CM Center point of pattern
A
Starting angle
Wi
Angle increment
K
Pattern diameter
W
End angle
V
Rotation direction (default: 0)
 VD=0, without W: Figures are arranged on a full circle
 VD=0, with W: Figures are arranged on the longer
circular arc
 VD=0, with Wi: The algebraic sign of Wi defines the
direction (Wi<0: clockwise)
 VD=1, with W: Clockwise
 VD=1, with Wi: Clockwise (algebraic sign of Wi has no
effect)
 VD=2, with W: Counterclockwise
 VD=2, with Wi: Counterclockwise (algebraic sign of Wi
has no effect)
Cycle form
X1
Milling top edge (diameter value)
X2
Milling floor (diameter value)
L
Slot length
A1
Angle to Z axis
P
Maximum infeed
FZ
Infeed rate
Further forms: see page 60
Access to the technology database:
 Machining operation: Milling
 Affected parameters: F, S, FZ, P
HEIDENHAIN MANUALplus 620, CNC PILOT 640
149
2.10 Units—Milling, lateral surface
"Helical slot milling" unit
The unit mills a helical slot. The slot width equals the diameter of the
milling cutter.
Unit name: G798_Wendelnut_C / Cycle: G798 (see page 357)
Position form
X1
Thread diameter
C1
Starting angle
Z1
Starting point of thread
Z2
End point of thread
U
Thread depth
Cycle form
F1
Thread pitch
J
Direction of thread:
 0: Right-hand thread
 1: Left-hand thread
D
No. of gears (threads per unit)
P
Run-in length
K
Run-out length
I
Maximum infeed
E
Cutting depth reduction
Further forms: see page 60
Access to the technology database:
 Machining operation: Finish milling
 Affected parameters: F, S
150
smart.Turn units
2.10 Units—Milling, lateral surface
"Contour milling, figures, lateral surface" unit
The unit mills the contour defined by Q on the lateral surface.
Unit name: G840_Fig_Mant_C / Cycle: G840 (see page 361)
Figure form
Q
Type of figure
QN
Z1
C1
CY
X1
P2
L
 0: Full circle
 1: Linear slot
 2: Circular slot
 3: Triangle
 4: Rectangle, square
 5: Polygon
Number of polygon corners—only with Q=5 (polygon)
Figure center
Angle of figure center
Figure center of unrolled lateral surface
Milling top edge
Depth of figure
Edge length / width across flats
B
RE
A
Q2
 L>0: Edge length
 L<0: Width across flats (inside diameter) for polygon
Rectangle width
Rounding radius
Angle to Z axis
Rotational direction of slot —only if Q=2 (circular slot)
W
 cw: In clockwise direction
 ccw: In counterclockwise direction
Angle of slot end point—only if Q=2 (circular slot)
Program only the parameters relevant to the selected
figure type.
Access to the technology database:
 Machining operation: Milling
 Affected parameters: F, S, FZ, P
HEIDENHAIN MANUALplus 620, CNC PILOT 640
151
2.10 Units—Milling, lateral surface
Cycle form
JK
Cutter position
H
 0: On the contour
 1: Within the contour
 2: Outside the contour
Cutting direction
P
I
K
FZ
E
R
O
 0: Up-cut milling
 1: Climb milling
Maximum infeed
Infeed-direction oversize
Contour-parallel oversize
Infeed rate
Reduced feed rate
Approach radius
Plunging behavior
NF
 0: Straight (vertical plunge)—The cycle moves the tool to
the starting point; the tool plunges at feed rate and mills
the contour.
 1: In predrilling—The cycle positions the tool above the
hole; the tool plunges and mills the contour.
Position mark (only if O=1)
"Global" form
RB
Retraction plane
Further parameters: see page 64
Further forms: see page 60
152
smart.Turn units
2.10 Units—Milling, lateral surface
"ICP contour milling, lateral surface" unit
The unit mills the contour defined with ICP on the lateral surface.
Unit name: G840_Kon_C_Mant / Cycle: G840 (see page 361)
Contour form
FK
see page 62
NS
Starting block no. of contour
NE
End block no. of contour
X1
Milling top edge (diameter value)
P2
Depth of contour (radius value)
Cycle form
JK
Cutter position
H
 0: On the contour
 1, closed contour: Within the contour
 1, open contour: Left of the contour
 2, closed contour: Outside the contour
 2, open contour: Right of the contour
 3: Depending on H and MD
Cutting direction
P
I
K
FZ
E
R
O
 0: Up-cut milling
 1: Climb milling
Maximum infeed
Contour-parallel oversize
Infeed-direction oversize
Infeed rate
Reduced feed rate
Approach radius
Plunging behavior
 0: Straight (vertical plunge)—The cycle moves the tool to
the starting point; the tool plunges at feed rate and mills
the contour.
 1: In predrilling—The cycle positions the tool above the
hole; the tool plunges and mills the contour.
NF
Position mark (only if O=1)
RB
Retraction plane (diameter value)
Further forms: see page 60
Access to the technology database:
 Machining operation: Finish milling
 Affected parameters: F, S, FZ, P
HEIDENHAIN MANUALplus 620, CNC PILOT 640
153
2.10 Units—Milling, lateral surface
"Pocket milling, figures, lateral surface" unit
The unit mills the pocket defined by Q. In QK, select the machining
operation (roughing/finishing) and the plunging strategy.
Unit name: G84x_Fig_Mant_C / Cycles: G845 (see page 370); G846
(see page 374)
Figure form
Q
Type of figure
QN
Z1
C1
CY
X1
P2
L
 0: Full circle
 1: Linear slot
 2: Circular slot
 3: Triangle
 4: Rectangle, square
 5: Polygon
Number of polygon corners—only with Q=5 (polygon)
Figure center
Angle of figure center
Figure center of unrolled lateral surface
Milling top edge
Depth of figure
Edge length / width across flats
B
RE
A
Q2
 L>0: Edge length
 L<0: Width across flats (inside diameter) for polygon
Rectangle width
Rounding radius
Angle to Z axis
Rotational direction of slot—only if Q=2 (circular slot)
W
 cw: In clockwise direction
 ccw: In counterclockwise direction
Angle of slot end point—only if Q=2 (circular slot)
Program only the parameters relevant to the selected
figure type.
Access to the technology database:
 Machining operation: Milling
 Affected parameters: F, S, FZ, P
154
smart.Turn units
2.10 Units—Milling, lateral surface
Cycle form
QK
Machining operation and plunging strategy
JT
 0: Roughing
 1: Finishing
 2: Helical roughing, manual
 3: Helical roughing, automatic
 4: Reciprocating linear roughing, manual
 5: Reciprocating linear roughing, automatic
 6: Reciprocating circular roughing, manual
 7: Reciprocating circular roughing, automatic
 8: Plunge roughing at predrilling position
 9: Finishing with 3-D approach arc
Machining direction:
H
 0: From the inside out (from the inside towards the
outside)
 1: From the outside in (from the outside towards the
inside)
Cutting direction
P
I
K
FZ
E
R
WB
EW
NF
U
 0: Up-cut milling
 1: Climb milling
Maximum infeed
Infeed-direction oversize
Contour-parallel oversize
Infeed rate
Reduced feed rate
Approach radius
Plunging length
Plunge angle
Position mark (only if QK=8)
Overlap factor (default: 0.5)
"Global" form
RB
Retraction plane
Further parameters: see page 64
Further forms: see page 60
HEIDENHAIN MANUALplus 620, CNC PILOT 640
155
2.10 Units—Milling, lateral surface
"ICP pocket milling, lateral surface" unit
The unit mills the pocket defined by Q. In QK, select the machining
operation (roughing/finishing) and the plunging strategy.
Unit name: G845_Tas_C_Mant / Cycles: G845 (see page 370); G846
(see page 374)
Contour form
FK
see page 62
NS
Starting block no. of contour
NE
End block no. of contour
X1
Milling top edge (diameter value)
P2
Depth of contour
NF
Position mark (only if QK=8)
Cycle form
QK
Machining operation and plunging strategy
JT
 0: Roughing
 1: Finishing
 2: Helical roughing, manual
 3: Helical roughing, automatic
 4: Reciprocating linear roughing, manual
 5: Reciprocating linear roughing, automatic
 6: Reciprocating circular roughing, manual
 7: Reciprocating circular roughing, automatic
 8: Plunge roughing at predrilling position
 9: Finishing with 3-D approach arc
Machining direction
H
 0: From the inside out (from the inside towards the
outside)
 1: From the outside in (from the outside towards the
inside)
Cutting direction
 0: Up-cut milling
 1: Climb milling
P
Maximum infeed
I
Infeed-direction oversize
K
Contour-parallel oversize
FZ
Infeed factor
E
Reduced feed rate
R
Approach radius
WB
Plunging length
EW
Plunge angle
U
Overlap factor (default: 0.5)
RB
Retraction plane (diameter value)
Further forms: see page 60
156
Access to the technology database:
 Machining operation: Milling
 Affected parameters: F, S, FZ, P
smart.Turn units
2.10 Units—Milling, lateral surface
"Engraving, lateral surface" unit
The unit engraves character strings aligned linearly on the lateral
surface. Diacritics and special characters that you cannot enter in the
smart.Turn editor can be defined, character by character, in NF. If you
program "Continue from last text" (Q=1), tool change and prepositioning are suppressed. The technological data of the previous
engraving cycle apply.
Unit name: G802_GRA_MANT_C / Cycle: G802 (see page 379)
Character set: see page 376
Position form
Z
Starting point
C
Starting angle
CY
Starting point
X
End point (diameter). X position, infeed depth during
milling.
RB
Retraction plane
Cycle form
TXT
Text to be engraved
NF
Character number (character to be engraved)
H
Font height
E
Distance factor (for calculation see figure)
W
Inclination angle
FZ
Plunging feed rate factor (plunging feed rate = current feed
rate * FZ)
D
Reference diameter
Q
Continue from last text
 0 (No): Engraving starts at the starting point
 1 (Yes): Engraving starts at the tool position
Further forms: see page 60
Access to the technology database:
 Machining operation: Engraving
 Affected parameters: F, S
HEIDENHAIN MANUALplus 620, CNC PILOT 640
157
2.10 Units—Milling, lateral surface
"Deburring, lateral surface" unit
The unit deburrs the contour defined with ICP on the lateral surface.
Unit name: G840_ENT_C_MANT / Cycle: G840 (see page 365)
Contour form
FK
see page 62
NS
Starting block no. of contour
NE
End block no. of contour
X1
Milling top edge (diameter value)
Cycle form
JK
Cutter position
H
 JK=0: On the contour
 JK=1, closed contour: Within the contour
 JK=1, open contour: Left of the contour
 JK=2, closed contour: Outside the contour
 JK=2, open contour: Right of the contour
 JK=3: Depending on H and MD
Cutting direction
 0: Up-cut milling
 1: Climb milling
BG
Chamfer width
JG
Preparation diameter
P
Plunging depth (indicated as a negative value)
K
Contour-parallel oversize
R
Approach radius
FZ
Infeed rate
E
Reduced feed rate
RB
Retraction plane
Further forms: see page 60
Access to the technology database:
 Machining operation: Deburring
 Affected parameters: F, S
158
smart.Turn units
"Program beginning (START)" unit
In the start unit, default values that are used in the following units are
defined. The start unit is called once at the beginning of the machining
section. You also directly specify the rotational speed limits, zero point
shift and tool change point for the program.
Unit name: Start / Called cycle: None
"Limits" form
S0
Maximum main spindle speed
S1
Maximum rotational speed of driven tool
Z
Zero point shift (G59)
"TC point" form (tool change point)
WT1
Tool change point
WX1
WZ1
WY1
Soft keys in the program beginning form
Loads the zero point defined during
setup
Loads the tool-change point defined
during setup
 No axis (do not approach the tool change point)
 0: Simultaneous (X and Z axes depart diagonally)
 1: First X, then Z
 2: First Z, then X
 3: Only X
 4: Only Z
 5: Only Y
 6: Simultaneous with Y
Tool change point in X (reference: distance of the slide
position as radius value from the machine zero point)
Tool change point in Z (reference: distance of the slide
position from the machine zero point)
Tool change point in Y (reference: distance of the slide
position from the machine zero point)
HEIDENHAIN MANUALplus 620, CNC PILOT 640
159
2.11 Units—Special operations
2.11 Units—Special operations
2.11 Units—Special operations
"Defaults" form
GWW
Tool change point
CLT
 No axis (do not approach the tool change point)
 0: Simultaneous (X and Z axes depart diagonally)
 1: First X, then Z
 2: First Z, then X
 3: Only X
 4: Only Z
 5: Only Y
 6: Simultaneous with Y
Coolant
G60
 0: Without
 1: Circuit 1 on
 2: Circuit 2 on
Protection zone (default for drilling units)
 0: Active
 1: Inactive
Cycle form
L
Subprogram name: Name of a subprogram that is called by
the start unit
"Global" form
G47
Safety clearance
SCK
Safety clearance in infeed direction (drilling and milling)
SCI
Safety clearance in the working plane (milling)
I, K
Oversize in X, Z direction (X: diameter value)
You can load the zero point shift and the tool change point
by soft key (see soft-key table).
 The setting in the "TC point" form applies only within the
current program.
 Position of tool change point (WX1, WZ1, WY1):
 If the tool change point is defined, you use G14 to
move to this position.
 If the tool change point is not defined, you use G14 to
move to the position defined in manual mode.
If you call a subprogram using the start unit, you should set
the subprogram with G65 Chuck selection with fixture D0.
You should also move the C axes out, for example with
M15 or M315.
160
smart.Turn units
2.11 Units—Special operations
"C axis ON" unit
The unit activates the SPI (spindle) C axis.
Unit name: C_Axis_ON / Called cycle: None
"C axis ON" form
SPI
Workpiece spindle number (0 to 3). Spindle that rotates the
workpiece.
C
Approach position
"C axis OFF" unit
The unit deactivates the SPI (spindle) C axis.
Unit name: C_Axis_OFF / Called cycle: None
"C axis OFF" form
SPI
Workpiece spindle number (0 to 3). Spindle that rotates the
workpiece.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
161
2.11 Units—Special operations
"Subprogram call" unit
The unit calls the subprogram defined in "L".
Access to the technology database:
Unit name: SUBPROG / Called cycle: Any subprogram
 Not possible
Contour form
L
Subprogram name
Q
Number of repetitions
LA-LF
Transfer values
LH
Transfer value
LN
Transfer value—reference to a block number as contour
reference. Is updated during block numbering.
Cycle form
LI-LK
Transfer values
LO
Transfer value
LP
Transfer value
LR
Transfer value
LS
Transfer value
LU
Transfer value
LW-LZ Transfer values
Cycle form
ID1
Transfer value—text variable (string)
AT1
Transfer value—text variable (string)
BS
Transfer value
BE
Transfer value
WS
Transfer value
AC
Transfer value
WC
Transfer value
RC
Transfer value
IC
Transfer value
KC
Transfer value
JC
Transfer value
 The tool call is not a mandatory parameter in this unit!
 Instead of the text "transfer value," texts can be
displayed that were defined in the subprogram. You can
also define help graphics for every line of the
subprogram (see page 427).
162
smart.Turn units
2.11 Units—Special operations
"Program section repeat" unit
Use the Repeat unit to program a program section repeat. The unit
consists of two inseparable parts. Program the unit with the Start form
immediately before the repeatable part, and the unit with the End form
immediately behind the repeatable part. Be sure to use the same
variable number here.
Unit name: REPEAT / Called cycle: None
"Start" form
AE
Repetition
V
NN
QR
 0: Start
 1: End
Variable number 1–30 (counting variable for the iteration
loop)
Number of repetitions
Save workpiece blank
 0: No
 1: Yes
K
Comment
"End" form
AE
Repetition:
V
Z
C
Q
K
 0: Start
 1: End
Variable number 1–30 (counting variable for the iteration
loop)
Additive zero point shift
Incremental shift, C axis
Number of the C axis
Comment
HEIDENHAIN MANUALplus 620, CNC PILOT 640
163
2.11 Units—Special operations
"Program end" unit
In every smart.Turn program, the end unit should be called once at the
end of the machining section.
Unit name: END / Called cycle: None
"Program end" form
ME
Type of return jump
NS
G14
 30: Without M30 restart
 99: With M99 restart
Block number for return jump
Tool change point
MFS
MFE
 No axis (do not approach the tool change point)
 0: Simultaneous (X and Z axes depart diagonally)
 1: First X, then Z
 2: First Z, then X
 3: Only X
 4: Only Z
 5: Only Y
 6: Simultaneous with Y
M command at the start of the unit
M command at the end of the unit
164
smart.Turn units
2.11 Units—Special operations
"Tilt plane" unit
The unit executes the following transformations and rotations:
 Shifts the coordinate system to the position I, K
 Rotates the coordinate system by the angle B; reference point: I, K
 Shifts, if programmed, the coordinate system by U and W in the
rotated coordinate system
Unit name: G16_ROTWORKPLAN / Called cycle: G16 (see page 522)
"Tilt plane" form
Q
Tilt plane
B
I
K
U
W
 0: OFF (disable tilting)
 1: ON (tilt working plane)
Angle: Plane angle (reference: positive Z axis)
Reference point: Plane reference in X direction (radius)
Reference point: Plane reference in Z direction
Shift in X: Shift in X direction
Shift in Z: Shift in Z direction
Please note:
 Q0 resets the working plane. The zero point and
coordinate system defined before the unit are then in
effect again.
 The positive Z axis is the reference axis for the "plane
angle B." This also applies to a mirrored coordinate
system.
 X is the infeed axis in a tilted coordinate system. X
coordinates are entered as diameter coordinates.
 Other zero point shifts are not permitted while tilting is
active.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
165
166
smart.Turn units
2.11 Units—Special operations
smart.Turn units for
the Y axis
3.1 Units—Drilling in the Y axis
3.1 Units—Drilling in the Y axis
"ICP drilling, Y axis" unit
The unit machines a single hole or a hole pattern in the XY or YZ plane.
Using ICP, you define the holes as well as further details.
Unit name: G74_ICP_Y / Cycle: G74 (see page 331)
Parameters on the Pattern form
FK
see page 62
NS
Starting block no. of contour
Parameters on the Cycle form
E
Delay (dwell time at end of hole) (default: 0)
D
Retraction at
V
 0: Rapid traverse
 1: Feed rate
Feed rate reduction
 0: Without reduction
 1: At end of the hole
 2: At start of the hole
 3: At start and end of the hole
AB
Spot drilling / through drilling length (distance for feed rate
reduction)
P
First hole depth
IB
Hole depth reduction value
JB
Minimum hole depth
B
Retraction distance
RI
Internal safety clearance: Distance for reapproach inside
the hole (default: safety clearance SCK).
RB
Retraction plane (default: return to the starting position or
to the safety clearance)
Further forms: see page 60
Access to the technology database:
 Machining operation: Drilling
 Affected parameters: F, S
168
smart.Turn units for the Y axis
3.1 Units—Drilling in the Y axis
"ICP tapping, Y axis" unit
The unit machines a single tap hole or a hole pattern in the XY or YZ
plane. Using ICP, you define the tap holes as well as further details.
Unit name: G73_ICP_Y / Cycle: G73 (see page 328)
Parameters on the Pattern form
FK
see page 62
NS
Starting block no. of contour
Parameters on the Cycle form
F1
Thread pitch
B
Run-in length
L
Retraction length when using floating tap holders (default: 0)
SR
Retraction speed (default: Shaft speed for tapping)
SP
Chip breaking depth
SI
Retraction distance
RB
Retraction plane
Further forms: see page 60
Retraction length L: Use this parameter for floating tap holders. The
cycle calculates a new nominal pitch on the basis of the thread depth,
the programmed pitch, and the "retraction length." The nominal pitch
is somewhat smaller than the pitch of the tap. During tapping, the tap
is pulled away from the chuck by the retraction length. With this
method you can achieve higher service life from the taps.
Access to the technology database:
 Machining operation: Tapping
 Affected parameters: S
HEIDENHAIN MANUALplus 620, CNC PILOT 640
169
3.1 Units—Drilling in the Y axis
"ICP boring/countersinking, Y axis" unit
The unit machines a single hole or a hole pattern in the XY or YZ plane.
Using ICP, you define the hole positions as well as further details for
boring or countersinking.
Unit name: G72_ICP_Y / Cycle: G72 (see page 327)
Parameters on the Pattern form
FK
see page 62
NS
Starting block no. of contour
Parameters on the Cycle form
E
Delay (dwell time at end of hole) (default: 0)
D
Retraction at
 0: Rapid traverse
 1: Feed rate
RB
Retraction plane (default: return to the starting position or
to the safety clearance)
Further forms: see page 60
Access to the technology database:
 Machining operation: Drilling
 Affected parameters: F, S
170
smart.Turn units for the Y axis
3.2 Units—Predrilling in Y axis
3.2 Units—Predrilling in Y axis
"Predrill, contour mill, ICP in XY plane" unit
The unit determines the hole position and machines the hole. The
subsequent milling cycle obtains the hole position from the reference
stored in NF. If the milling contour consists of multiple sections, the
unit machines a hole for each section.
Unit name: DRILL_STI_840_Y / Cycles: G840 A1 (see page 359); G71
(see page 325)
Parameters on the Contour form
FK
see page 62
NS
Starting block no. of contour
NE
End block no. of contour
Z1
Milling top edge
P2
Depth of contour
Parameters on the Cycle form
JK
Cutter position
H
 0: On the contour
 1, closed contour: Within the contour
 1, open contour: Left of the contour
 2, closed contour: Outside the contour
 2, open contour: Right of the contour
 3: Depending on H and MD
Cutting direction
I
K
R
WB
NF
E
D
 0: Up-cut milling
 1: Climb milling
Contour-parallel oversize
Infeed-direction oversize
Approach radius
Cutter diameter
Position mark
Delay (dwell time at end of hole) (default: 0)
Retraction at
V
 0: Rapid traverse
 1: Feed rate
Feed rate reduction
Access to the technology database:
 Machining operation: Drilling
 Affected parameters: F, S
 0: Without reduction
 1: At end of the hole
 2: At start of the hole
 3: At start and end of the hole
AB
Spot drilling / through drilling length (distance for feed rate
reduction)
RB
Retraction plane (default: return to the starting position or
to the safety clearance)
Further forms: see page 60
HEIDENHAIN MANUALplus 620, CNC PILOT 640
171
3.2 Units—Predrilling in Y axis
"Predrill, pocket mill, ICP in XY plane" unit
The unit determines the hole position and machines the hole. The
subsequent milling cycle obtains the hole position from the reference
stored in NF. If the pocket consists of multiple sections, the unit
machines a hole for each section.
Unit name: DRILL_STI_845_Y / Cycles: G845 A1 (see page 369); G71
(see page 325)
Parameters on the Contour form
FK
see page 62
NS
Starting block no. of contour
NE
End block no. of contour
Z1
Milling top edge
P2
Depth of contour
Parameters on the Cycle form
JT
Machining direction:
H
 0: From the inside out (from the inside towards the
outside)
 1: From the outside in (from the outside towards the
inside)
Cutting direction
I
K
U
WB
NF
E
D
 0: Up-cut milling
 1: Climb milling
Contour-parallel oversize
Infeed-direction oversize
Overlap factor (default: 0.5)
Cutter diameter
Position mark
Delay (dwell time at end of hole) (default: 0)
Retraction at
V
 0: Rapid traverse
 1: Feed rate
Feed rate reduction
 0: Without reduction
 1: At end of the hole
 2: At start of the hole
 3: At start and end of the hole
AB
Spot drilling / through drilling length (distance for feed rate
reduction)
RB
Retraction plane (default: return to the starting position or
to the safety clearance)
Further forms: see page 60
Access to the technology database:
 Machining operation: Drilling
 Affected parameters: F, S
172
smart.Turn units for the Y axis
3.2 Units—Predrilling in Y axis
"Predrill, contour mill, ICP in YZ plane" unit
The unit determines the hole position and machines the hole. The
subsequent milling cycle obtains the hole position from the reference
stored in NF. If the milling contour consists of multiple sections, the
unit machines a hole for each section.
Unit name: DRILL_MAN_840_Y / Cycles: G840 A1 (see page 359);
G71 (see page 325)
Parameters on the Contour form
FK
see page 62
NS
Starting block no. of contour
NE
End block no. of contour
X1
Milling top edge (diameter value)
P2
Depth of contour (radius value)
Parameters on the Cycle form
JK
Cutter position
H
 JK=0: On the contour
 JK=1, closed contour: Within the contour
 JK=1, open contour: Left of the contour
 JK=2, closed contour: Outside the contour
 JK=2, open contour: Right of the contour
 JK=3: Depending on H and MD
Cutting direction
I
K
R
WB
NF
E
D
 0: Up-cut milling
 1: Climb milling
Contour-parallel oversize
Infeed-direction oversize
Approach radius
Cutter diameter
Position mark
Delay (dwell time at end of hole) (default: 0)
Retraction at
V
 0: Rapid traverse
 1: Feed rate
Feed rate reduction
 0: Without reduction
 1: At end of the hole
 2: At start of the hole
 3: At start and end of the hole
AB
Spot drilling / through drilling length (distance for feed rate
reduction)
RB
Retraction plane (diameter value)
Further forms: see page 60
HEIDENHAIN MANUALplus 620, CNC PILOT 640
Access to the technology database:
 Machining operation: Drilling
 Affected parameters: F, S
173
3.2 Units—Predrilling in Y axis
"Predrill, pocket mill, ICP in YZ plane" unit
The unit determines the hole position and machines the hole. The
subsequent milling cycle obtains the hole position from the reference
stored in NF. If the pocket consists of multiple sections, the unit
machines a hole for each section.
Unit name: DRILL_MAN_845_Y / Cycles: G845 A1 (see page 369)
Parameters on the Contour form
FK
see page 62
NS
Starting block no. of contour
NE
End block no. of contour
X1
Milling top edge (diameter value)
P2
Depth of contour
Parameters on the Cycle form
JT
Machining direction:
H
 0: From the inside out (from the inside towards the
outside)
 1: From the outside in (from the outside towards the
inside)
Cutting direction
P
I
K
U
WB
NF
E
D
 0: Up-cut milling
 1: Climb milling
Maximum infeed
Infeed-direction oversize
Contour-parallel oversize
Overlap factor (default: 0.5)
Cutter diameter
Position mark
Delay (dwell time at end of hole) (default: 0)
Retraction at
V
 0: Rapid traverse
 1: Feed rate
Feed rate reduction
 0: Without reduction
 1: At end of the hole
 2: At start of the hole
 3: At start and end of the hole
AB
Spot drilling / through drilling length (distance for feed rate
reduction)
RB
Retraction plane (diameter value)
Further forms: see page 60
Access to the technology database:
 Machining operation: Drilling
 Affected parameters: F, S
174
smart.Turn units for the Y axis
3.3 Units—Milling in Y axis
3.3 Units—Milling in Y axis
"ICP contour milling in XY plane" unit
The unit mills the contour defined with ICP in the XY plane.
Unit name: G840_Kon_Y_Stirn / Cycle: G840 (see page 361)
Parameters on the Contour form
FK
see page 62
NS
Starting block no. of contour
NE
End block no. of contour
Z1
Milling top edge
P2
Depth of contour
Parameters on the Cycle form
JK
Cutter position
H
 JK=0: On the contour
 JK=1, closed contour: Within the contour
 JK=1, open contour: Left of the contour
 JK=2, closed contour: Outside the contour
 JK=2, open contour: Right of the contour
 JK=3: Depending on H and MD
Cutting direction
P
I
K
FZ
E
R
O
 0: Up-cut milling
 1: Climb milling
Maximum infeed
Contour-parallel oversize
Infeed-direction oversize
Infeed rate
Reduced feed rate
Approach radius
Plunging behavior
 0: Straight (vertical plunge)—The cycle moves the tool to
the starting point; the tool plunges at feed rate and mills
the contour.
 1: In predrilling—The cycle positions the tool above the
hole; the tool plunges and mills the contour.
NF
Position mark (only if O=1)
RB
Retraction plane
Further forms: see page 60
Access to the technology database:
 Machining operation: Finish milling
 Affected parameters: F, S, FZ, P
HEIDENHAIN MANUALplus 620, CNC PILOT 640
175
3.3 Units—Milling in Y axis
"ICP pocket milling in XY plane" unit
The unit mills the pocket defined with ICP in the XY plane. In QK
(machining operation), select whether a roughing or finishing
operation is to be executed. For roughing, define the plunging
strategy.
Unit name: G845_Tas_Y_Stirn / Cycles: G845 (see page 370); G846
(see page 374)
Parameters on the Contour form
FK
see page 62
NF
Position mark (only if QK=8)
NS
Starting block no. of contour
Z1
Milling top edge
P2
Depth of contour
NE
End block no. of contour
Parameters on the Cycle form
QK
Machining operation and plunging strategy
JT
 0: Roughing
 1: Finishing
 2: Helical roughing, manual
 3: Helical roughing, automatic
 4: Reciprocating linear roughing, manual
 5: Reciprocating linear roughing, automatic
 6: Reciprocating circular roughing, manual
 7: Reciprocating circular roughing, automatic
 8: Plunge roughing at predrilling position
 9: Finishing with 3-D approach arc
Machining direction:
H
 0: From the inside out (from the inside towards the
outside)
 1: From the outside in (from the outside towards the
inside)
Cutting direction
 0: Up-cut milling
 1: Climb milling
P
Maximum infeed
I
Contour-parallel oversize
K
Infeed-direction oversize
FZ
Infeed rate
E
Reduced feed rate
R
Approach radius
WB
Plunging length
EW
Plunge angle
U
Overlap factor (default: 0.5)
RB
Retraction plane
Further forms: see page 60
176
Access to the technology database:
 Machining operation: Milling
 Affected parameters: F, S, FZ, P
smart.Turn units for the Y axis
3.3 Units—Milling in Y axis
"Single-surface milling, XY plane" unit
The unit mills a single surface defined with ICP in the XY plane.
Unit name: G841_Y_STI / Cycles: G841 (see page 527); G842 (see
page 528)
Parameters on the Contour form
FK
see page 62
NS
Starting block no. of contour
Parameters on the Cycle form
QK
Machining operation:
P
I
K
H
 0: Roughing
 1: Finishing
Maximum infeed
Contour-parallel oversize
Infeed-direction oversize
Cutting direction
 0: Up-cut milling
 1: Climb milling
U
Overlap factor (default: 0.5)
V
Overrun factor
FZ
Infeed rate
RB
Retraction plane
Further forms: see page 60
Access to the technology database:
 Machining operation: Milling
 Affected parameters: F, S, FZ, P
HEIDENHAIN MANUALplus 620, CNC PILOT 640
177
3.3 Units—Milling in Y axis
"Centric polygon milling, XY plane" unit
The unit mills the centric polygon defined with ICP in the XY plane.
Unit name: G843_Y_STI / Cycles: G843 (see page 529); G844 (see
page 530)
Parameters on the Contour form
FK
see page 62
NS
Starting block no. of contour
Parameters on the Cycle form
QK
Machining operation:
P
I
K
H
 0: Roughing
 1: Finishing
Maximum infeed
Contour-parallel oversize
Infeed-direction oversize
Cutting direction
 0: Up-cut milling
 1: Climb milling
U
Overlap factor (default: 0.5)
V
Overrun factor
FZ
Infeed rate
RB
Retraction plane
Further forms: see page 60
Access to the technology database:
 Machining operation: Milling
 Affected parameters: F, S, FZ, P
178
smart.Turn units for the Y axis
3.3 Units—Milling in Y axis
"Engraving in XY plane" unit
The unit engraves character strings aligned linearly in the XY plane.
Diacritics and special characters that you cannot enter in the
smart.Turn editor can be defined, character by character, in NF. If you
program "Continue from last text" (Q=1), tool change and prepositioning are suppressed. The technological data of the previous
engraving cycle apply.
Unit name: G803_GRA_Y_STIRN / Cycle: G803 (see page 539)
Character set: see page 376
Parameters on the Position form
X, Y
Starting point
Z
End point. Z position, infeed depth during milling.
RB
Retraction plane
APP
Approach: see page 65
DEP
Departure: see page 65
Parameters on the Cycle form
TXT
Text to be engraved
NF
Character number (character to be engraved)
H
Font height
E
Distance factor (for calculation see figure)
W
Inclination angle
FZ
Plunging feed rate factor (plunging feed rate = current feed
rate * FZ)
Q
Continue from last text
 0 (No): Engraving starts at the starting point
 1 (Yes): Engraving starts at the tool position
Further forms: see page 60
Access to the technology database:
 Machining operation: Engraving
 Affected parameters: F, S
HEIDENHAIN MANUALplus 620, CNC PILOT 640
179
3.3 Units—Milling in Y axis
"Deburring in XY plane" unit
The unit deburrs the contour defined with ICP in the XY plane.
Unit name: G840_ENT_Y_STIRN / Cycle: G840 (see page 365)
Parameters on the Contour form
FK
see page 62
NS
Starting block no. of contour
NE
End block no. of contour
Z1
Milling top edge
Parameters on the Cycle form
JK
Cutter position
H
 JK=0: On the contour
 JK=1, closed contour: Within the contour
 JK=1, open contour: Left of the contour
 JK=2, closed contour: Outside the contour
 JK=2, open contour: Right of the contour
 JK=3: Depending on H and MD
Cutting direction
 0: Up-cut milling
 1: Climb milling
BG
Chamfer width
JG
Preparation diameter
P
Plunging depth (indicated as a negative value)
I
Contour-parallel oversize
R
Approach radius
FZ
Infeed rate
E
Reduced feed rate
RB
Retraction plane
Further forms: see page 60
Access to the technology database:
 Machining operation: Deburring
 Affected parameters: F, S
180
smart.Turn units for the Y axis
3.3 Units—Milling in Y axis
"Thread milling in XY plane" unit
The unit mills a thread in existing holes in the XY plane.
Unit name: G800_GEW_Y_STIRN / Cycle: G800 (see page 541)
Parameters on the Position form
APP
Approach see page 65
CS
Approach position C
Z1
Start point drill (starting point of hole)
P2
Thread depth
I
Thread diameter
F1
Thread pitch
Parameters on the Cycle form
J
Direction of thread:
H
 0: Right-hand thread
 1: Left-hand thread
Cutting direction
V
 0: Up-cut milling
 1: Climb milling
Milling method
 0: The thread is milled in a 360-degree helix
 1: The thread is milled in several helical paths (singlepoint tool)
R
Approach radius
Further forms: see page 60
Access to the technology database:
 Machining operation: Finish milling
 Affected parameters: F, S
HEIDENHAIN MANUALplus 620, CNC PILOT 640
181
3.3 Units—Milling in Y axis
"ICP contour milling in YZ plane" unit
The unit mills the contour defined with ICP in the YZ plane.
Unit name: G840_Kon_Y_Mant / Cycle: G840 (see page 361)
Parameters on the Contour form
FK
see page 62
NS
Starting block no. of contour
NE
End block no. of contour
X1
Milling top edge (diameter value)
P2
Depth of contour (radius value)
Parameters on the Cycle form
JK
Cutter position
H
 JK=0: On the contour
 JK=1, closed contour: Within the contour
 JK=1, open contour: Left of the contour
 JK=2, closed contour: Outside the contour
 JK=2, open contour: Right of the contour
 JK=3: Depending on H and MD
Cutting direction
P
I
K
FZ
E
R
O
 0: Up-cut milling
 1: Climb milling
Maximum infeed
Contour-parallel oversize
Infeed-direction oversize
Infeed rate
Reduced feed rate
Approach radius
Plunging behavior
 0: Straight (vertical plunge)—The cycle moves the tool to
the starting point; the tool plunges at feed rate and mills
the contour.
 1: In predrilling—The cycle positions the tool above the
hole; the tool plunges and mills the contour.
NF
Position mark (only if O=1)
RB
Retraction plane (diameter value)
Further forms: see page 60
Access to the technology database:
 Machining operation: Finish milling
 Affected parameters: F, S, FZ, P
182
smart.Turn units for the Y axis
3.3 Units—Milling in Y axis
"ICP pocket milling in YZ plane" unit
The unit mills the pocket defined with ICP in the YZ plane. In QK
(machining operation), select whether a roughing or finishing
operation is to be executed. For roughing, define the plunging
strategy.
Unit name: G845_Tas_Y_Mant / Cycles: G845 (see page 370); G846
(see page 374)
Parameters on the Contour form
FK
see page 62
NS
Starting block no. of contour
NE
End block no. of contour
X1
Milling top edge (diameter value)
P2
Depth of contour
NF
Position mark (only if QK=8)
Parameters on the Cycle form
QK
Machining operation and plunging strategy
JT
 0: Roughing
 1: Finishing
 2: Helical roughing, manual
 3: Helical roughing, automatic
 4: Reciprocating linear roughing, manual
 5: Reciprocating linear roughing, automatic
 6: Reciprocating circular roughing, manual
 7: Reciprocating circular roughing, automatic
 8: Plunge roughing at predrilling position
 9: Finishing with 3-D approach arc
Machining direction:
H
 0: From the inside out (from the inside towards the
outside)
 1: From the outside in (from the outside towards the
inside)
Cutting direction
 0: Up-cut milling
 1: Climb milling
P
Maximum infeed
I
Infeed-direction oversize
K
Contour-parallel oversize
FZ
Infeed rate
E
Reduced feed rate
R
Approach radius
WB
Plunging length
EW
Plunge angle
U
Overlap factor (default: 0.5)
RB
Retraction plane (diameter value)
Further forms: see page 60
HEIDENHAIN MANUALplus 620, CNC PILOT 640
Access to the technology database:
 Machining operation: Milling
 Affected parameters: F, S, FZ, P
183
3.3 Units—Milling in Y axis
"Single-surface milling, YZ plane" unit
The unit mills a single surface defined with ICP in the YZ plane.
Unit name: G841_Y_MANT / Cycles: G841 (see page 527), G842 (see
page 528)
Parameters on the Contour form
FK
see page 62
NS
Starting block no. of contour
Parameters on the Cycle form
QK
Machining operation:
P
I
K
H
 0: Roughing
 1: Finishing
Maximum infeed
Contour-parallel oversize
Infeed-direction oversize
Cutting direction
 0: Up-cut milling
 1: Climb milling
U
Overlap factor (default: 0.5)
V
Overrun factor
FZ
Infeed rate
RB
Retraction plane
Further forms: see page 60
Access to the technology database:
 Machining operation: Milling
 Affected parameters: F, S, FZ, P
184
smart.Turn units for the Y axis
3.3 Units—Milling in Y axis
"Centric polygon milling, YZ plane" unit
The unit mills the centric polygon defined with ICP in the YZ plane.
Unit name: G843_Y_MANT / Cycles: G843 (see page 529); G844 (see
page 529)
Parameters on the Contour form
FK
see page 62
NS
Starting block no. of contour
Parameters on the Cycle form
QK
Machining operation:
P
I
K
H
 0: Roughing
 1: Finishing
Maximum infeed
Contour-parallel oversize
Infeed-direction oversize
Cutting direction
 0: Up-cut milling
 1: Climb milling
U
Overlap factor (default: 0.5)
V
Overrun factor
FZ
Infeed rate
RB
Retraction plane
Further forms: see page 60
Access to the technology database:
 Machining operation: Milling
 Affected parameters: F, S, FZ, P
HEIDENHAIN MANUALplus 620, CNC PILOT 640
185
3.3 Units—Milling in Y axis
"Engraving in YZ plane" unit
The unit engraves character strings aligned linearly in the YZ plane.
Diacritics and special characters that you cannot enter in the
smart.Turn editor can be defined, character by character, in NF. If you
program "Continue from last text" (Q=1), tool change and prepositioning are suppressed. The technological data of the previous
engraving cycle apply.
Unit name: G804_GRA_Y_MANT / Cycle: G804 (see page 540)
Character set: see page 376
Parameters on the Position form
Y, Z
Starting point
X
End point (diameter). X position, infeed depth during
milling.
RB
Retraction plane
Parameters on the Cycle form
TXT
Text to be engraved
NF
Character number (character to be engraved)
H
Font height
E
Distance factor (for calculation see figure)
W
Inclination angle
FZ
Plunging feed rate factor (plunging feed rate = current feed
rate * FZ)
Q
Continue from last text
 0 (No): Engraving starts at the starting point
 1 (Yes): Engraving starts at the tool position
Further forms: see page 60
Access to the technology database:
 Machining operation: Engraving
 Affected parameters: F, S
186
smart.Turn units for the Y axis
3.3 Units—Milling in Y axis
"Deburring in YZ plane" unit
The unit deburrs the contour defined with ICP in the YZ plane.
Unit name: G840_ENT_Y_MANT / Cycle: G840 (see page 365)
Parameters on the Contour form
FK
see page 62
NS
Starting block no. of contour
NE
End block no. of contour
X1
Milling top edge (diameter value)
Parameters on the Cycle form
JK
Cutter position
H
 JK=0: On the contour
 JK=1, closed contour: Within the contour
 JK=1, open contour: Left of the contour
 JK=2, closed contour: Outside the contour
 JK=2, open contour: Right of the contour
 JK=3: Depending on H and MD
Cutting direction
 0: Up-cut milling
 1: Climb milling
BG
Chamfer width
JG
Preparation diameter
P
Plunging depth (indicated as a negative value)
K
Contour-parallel oversize
R
Approach radius
FZ
Infeed rate
E
Reduced feed rate
RB
Retraction plane
Further forms: see page 60
Access to the technology database:
 Machining operation: Deburring
 Affected parameters: F, S
HEIDENHAIN MANUALplus 620, CNC PILOT 640
187
3.3 Units—Milling in Y axis
"Thread milling in YZ plane" unit
The unit mills a thread in existing holes in the YZ plane.
Unit name: G806_GEW_Y_MANT / Cycle: G806 (see page 542)
Parameters on the Position form
APP
Approach see page 65
CS
Approach position C
X1
Start point drill (starting point of hole)
P2
Thread depth
I
Thread diameter
F1
Thread pitch
Parameters on the Cycle form
J
Direction of thread:
H
 0: Right-hand thread
 1: Left-hand thread
Cutting direction
V
 0: Up-cut milling
 1: Climb milling
Milling method
 0: The thread is milled in a 360-degree helix
 1: The thread is milled in several helical paths (singlepoint tool)
R
Approach radius
Further forms: see page 60
Access to the technology database:
 Machining operation: Finish milling
 Affected parameters: F, S
188
smart.Turn units for the Y axis
DIN Programming
4.1 Programming in DIN/ISO mode
4.1 Programming in DIN/ISO mode
Geometry and machining commands
The Steuerung also supports structured programming in DIN/ISO
mode.
The G commands are divided into:
 Geometry commands for describing the blank and finished part.
 Machining commands for the MACHINING section.
Some G codes are used for blank/finished-part definition
and in the MACHINING section. When copying or shifting
NC blocks, keep in mind that "geometry" functions are
used exclusively for describing a contour, while
"machining" functions are used only in the MACHINING
section.
Beispiel: "Structured DINplus program"
HEADER
#MATERIAL
Steel
#MACHINE
Automatic lathe
#DRAWING
356_787.9
#CLAMP_PRESS.
20
#SLIDE
$1
#COMPANY
Turn & Co
#MEASURE_UNITS
METRIC
TURRET 1
T1 ID"342-300.1"
T2 ID"111-80-080.1"
...
BLANK
N1 G20 X120 Z120 K2
FINISHED
N2 G0 X60 Z-115
N3 G1 Z-105
...
MACHINING
N22 G59 Z282
N25 G14 Q0
[Predrilling 30 mm outside centric face]
N26 T1
N27 G97 S1061 G95 F0.25 M4
...
END
190
DIN Programming
4.1 Programming in DIN/ISO mode
Contour programming
The "contour follow-up" function and contour-related turning cycles
require the previous description of the blank and finished part. For
milling and drilling, contour definition is a precondition if you wish to
use fixed cycles.
Use ICP (Interactive Contour Programming) for describing
blank and finished parts.
Contours for turning:
 Describe a continuous contour.
 The direction of the contour description is independent of the
direction of machining.
 Contour descriptions must not extend beyond the turning center.
 The contour of the finished part must lie within the contour of the
blank part.
 When machining bars, define only the required section as blank.
 Contour definitions apply to the entire NC program, even if the
workpiece is rechucked for machining the rear face.
 In the fixed cycles, the defined contour is used to program
"reference values."
To describe workpiece blanks and auxiliary workpiece blanks, use
 G20 "Blank part macro" for standard parts (cylinder, hollow cylinder).
 G21 "Cast-part macro" for blank-part contours based on finished-part
contours. G21 is only used for describing workpiece blanks.
 Individual contour elements (such as are used for finished-part
contours) where use of G20 or G21 is not possible.
To describe finished parts, use individual contour elements and form
elements. The contour elements or the complete contour can be
assigned attributes accounted for during the machining of the
workpiece (example: oversizes, additive compensation, special feed
rates, etc.). The Steuerung always uses paraxial elements to close
finished parts.
For intermediate machining steps, define auxiliary contours.
Auxiliary contours are programmed in the same way as finished-part
descriptions. One contour description is possible per AUXILIARY
CONTOUR. An AUXILIARY CONTOUR is assigned a name (ID) that
can be referenced by the cycles. Auxiliary contours are not closed
automatically.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
191
4.1 Programming in DIN/ISO mode
Contours for C-axis machining:
 Contours for C-axis machining are programmed within the
FINISHED PART section.
 Identify the contours as FACE or LATERAL. You can use section
codes more than once or program multiple contours within one
section code.
Block references: When editing G commands related to the contour
(MACHINING section), load the block references from the displayed
contour.

Place the cursor in the input box (NS).
 Switch to the contour display.

Place the cursor on the desired contour element.

Switch to NE.

Place the cursor on the desired contour element.

Press the LOAD soft key to return to the dialog.
NC blocks of the DIN program
An NC block contains NC commands such as positioning, switching
or organizational commands. Traversing and switching commands
begin with G or M followed by a number (G1, G2, G81, M3, M30, ...)
and the address parameters. Organizational commands consist of key
words (WHILE, RETURN, etc.), or of a combination of letters/
numbers.
You can also program NC blocks containing only variable calculations.
You can program several NC commands in one NC block, provided
they have different address letters and do not have opposing
functions.
Examples
 Permissible combination: N10 G1 X100 Z2 M8
 Non-permissible combination:
N10 G1 X100 Z2 G2 X100 Z2 R30 (same address letters are used
more than once) or
N10 M3 M4 (opposing functionality)
NC address parameters
The address parameters consist of 1 or 2 letter(s) followed by
 A value
 A mathematical expression
 A question mark—simplified geometry programming (VGP)
 A letter "i" to designate incremental address parameters (examples:
Xi..., Ci..., XKi..., YKi..., etc.)
 A # variable
 A constant (_constname)
192
DIN Programming
4.1 Programming in DIN/ISO mode
Examples:
 X20 [Absolute dimension]
 Zi–35.675 [Incremental dimension]
 X? [Simplified geometry programming]
 X#l1 [Variable programming]
 X(#g12+1) [Variable programming]
 X(37+2)*SIN(30) [Mathematical expression]
 X(20*_pi) [Expression with constant]
Creating, editing and deleting NC blocks
Make NC block:


Press the INS key. The Steuerung creates a new NC
block below the cursor position.
Alternatively you can program the NC command directly. The
Steuerung creates a new NC block or inserts the NC command in
the existing NC block.
Delete the NC block:

Position the cursor on the NC block to be deleted.
 Press the DEL key. The Steuerung deletes the NC
block.
Add an NC element:


Position the cursor on an element of the NC block (NC block
number, G or M command, address parameter, etc.).
Insert NC element (G, M, T function, etc.).
Change NC element:

Position the cursor on an element of the NC block (NC block
number, G or M command, address parameter, etc.) or the section
code.
 Press ENTER or double-click with the left mouse
key. The Steuerung activates a dialog box which
displays the block number, the number of the G or M
function, or the address parameters, which can then
be edited.
Delete NC element:

Position the cursor on an element of the NC block (NC block
number, G or M command, address parameter, etc.).
 Press the DEL key. The NC element highlighted by the
cursor and all the related elements are deleted.
Example: If the cursor is located on a G command, the
address parameters are also deleted.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
193
4.1 Programming in DIN/ISO mode
Address parameters
Coordinates can be programmed absolutely or incrementally. If you do
not make any entry for X, Y, Z, XK, YK, C, the coordinates of the block
previously executed will be retained (modal).
The Steuerung calculates missing coordinates in the principal axes X,
Y or Z if you program "?" (simplified geometry programming).
The machining functions G0, G1, G2, G3, G12 and G13 are modal. This
means that the Steuerung uses the previous G command if the
address parameters X, Y, Z, I or K in the following block have been
programmed without a G code. However, the address parameters
must have been programmed as absolute values.
The Steuerung supports the use of variables and mathematical
expressions as address parameters.
To edit address parameters:



Call the dialog box.
Position the cursor in the input field and enter/change the values, or
Use the additional input options provided by the soft keys.
 Enter "?" (simplified geometry programming)
 Switch from incremental to absolute, or vice versa
 Activate variable input
 Load the contour reference
You can use simplified geometry programming when
target or center point coordinates are missing. Simplified
geometry programming provides the following options:
 ?: The control calculates the value.
 ?>: The control calculates the value. If there are two
possible solutions, the control uses the higher value.
 ?<: The control calculates the value. If there are two
possible solutions, the control uses the lower value.
194
Soft key in the G dialog
Alternately shows and hides the help
graphics
Opens the alphabetic keyboard for
entering variables (GOTO key)
Inserts the question mark for activating
the simplified geometry programming
Activates incremental programming for
the current input parameter
Allows transferring the contour
references for NS and NE
DIN Programming
4.1 Programming in DIN/ISO mode
Fixed cycles
HEIDENHAIN recommends programming a fixed cycle as follows:
 Insert the tool
 Define the cutting data
 Position the tool in front of the working area
 Define the safety clearance
 Cycle call
 Retract the tool
 Move to tool change point
Danger of collision!
Remember when omitting cycle programming steps
during optimization:
 A special feed rate remains in effect until the next feed
command (for example the finishing feed rate during
recessing cycles).
 Some cycles traverse diagonally back to the starting
point if you use the standard programming (for example
roughing cycles).
Typical structure of a fixed cycle
...
MACHINING
N.. G59 Z..
Zero point shift
N.. G26 S..
Define the speed limit
N.. G14 Q..
Move to tool change point
...
N.. T..
Insert the tool
N.. G96 S.. G95 F.. M4
Define the technology data
N.. G0 X.. Z..
Pre-position
N.. G47 P..
Define the safety clearance
N.. G810 NS.. NE..
Cycle call
N.. G0 X.. Z..
If necessary, retract
N.. G14 Q0
Move to tool change point
...
HEIDENHAIN MANUALplus 620, CNC PILOT 640
195
4.1 Programming in DIN/ISO mode
Subprograms, expert programs
Subprograms are used to program the contour or the machining
process.
In the subprogram, transfer parameters are available as variables. You
can fix the designation of the transfer parameters and illustrate them
in help graphics (See "Subprograms" on page 427.).
In every subprogram, the local variables #l1 to #l30 are available for
internal calculations.
Subprograms can be nested up to six times. Nesting means that a
subprogram calls a further subprogram, etc.
If a subprogram is to be run repeatedly, enter the number of times the
subprogram is to be repeated in the Q parameter.
The Steuerung distinguishes between local and external
subprograms.
 Local subprograms are in the file of the NC main program. Local
subprograms can only be called in from their corresponding main
programs.
 External subprograms are stored in separate NC files and can be
called in from any NC main program or other NC subprograms.
Expert programs
An expert program is a subprogram that executes complex processes
and is adapted to the machine configurations. Expert programs are
usually provided by the machine tool builder.
NC program conversion
For programming and user communication, keep in mind that the
Steuerung interprets the NC program up to the fixed word
MACHINING in the program selection. The MACHINING section is not
interpreted until you select Cycle on.
196
DIN Programming
4.1 Programming in DIN/ISO mode
DIN/ISO programs of predecessor controls
The DIN program formats of the predecessor controls MANUALplus
4110 and CNC PILOT 4290 differ from the format of the MANUALplus
620. However, you can use the program converter to adapt programs
of the predecessor control to the new control.
When opening an NC program, the Steuerung recognizes the
programs of predecessor controls. The program concerned will be
converted after a confirmation prompt. "CONV_..." will be prefixed to
the program name.
The converter is also part of the Transfer function (Organization mode
of operation).
DIN/ISO programs not only have new solutions for tool management,
technology data, etc., but also for contour description and variable
programming.
Remember the following when converting DIN/ISO programs of the
MANUALplus 4110:
 Tool call: The loading of the T number depends on whether the
program is a "multifix program" (2-digit T number) or "turret program"
(4-digit T number).
 2-digit T number: The T number is loaded as "ID" and entered as
the T number "T1".
 4-digit T number (Tddpp): The first two digits of the T number (dd)
are loaded as "ID" and the last two (pp) as "T".
 Workpiece-blank definition: A G20/G21 workpiece-blank
definition of the 4110 becomes an AUXILIARY BLANK.
 Contour descriptions: In MANUALplus 4110 programs, the fixed
cycles are followed by the contour description. During conversion
the contour description is converted to an AUXILIARY CONTOUR.
The associated cycle in the MACHINING section then refers to this
auxiliary contour.
 Variable programming: Variable accesses to tool data, machine
dimensions, D compensation values, parameter data and events
cannot be converted. These program sequences have to be
adapted.
 M functions are left unchanged.
 Inches or metric: The converter cannot detect the unit of measure
of the MANUALplus 4110 program. Consequently, no unit of
measure is entered in the target program. This has to be completed
by the user.
Remember the following when converting DIN programs of the CNC
PILOT 4290:
 Tool call (T commands of the TURRET section):
 T commands containing a reference to the tool database are left
unchanged (example: T1 ID"342-300.1").
 T commands containing tool data cannot be converted.
 Variable programming: Variable accesses to tool data, machine
dimensions, D compensation values, parameter data and events
cannot be converted. These program sequences have to be
adapted.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
197
4.1 Programming in DIN/ISO mode
 M functions are left unchanged.
 Names of external subprograms: When an external subprogram
is called, the converter prefixes "CONV_..." to the name.
If the DIN program contains nonconvertible elements, the
corresponding NC block is saved as a comment. The word
WARNING is inserted in front of this comment. Depending
on the situation, the nonconvertible command is taken into
the comment line, or the nonconvertible NC block follows
the comment.
HEIDENHAIN recommends adapting converted NC
programs to the circumstances of the Steuerung and then
testing them before using them for production.
198
DIN Programming
4.1 Programming in DIN/ISO mode
"Geometry" pull-down menus
The Geo(metry) pull-down menus contain functions for contour
description. The pull-down menus are called by pressing the "Geo"
menu in DIN/ISO mode.
Overview of the functions:
 G: Direct entry of a G code
 Line: Direct entry of a line segment (G1)
 Circle: Description of a circular arc (G2, G3, G12, G13)
 Form: Description of form elements
 Front: Functions for contour descriptions on the front face
 Surface: Functions for contour descriptions on the lateral surface
 ICP, Extras, Graph.: See "Shared menu items" on page 41.

Back to the DIN/ISO main menu
"Machining" pull-down menus
The "Mach(ining)" pull-down menus contain functions for
programming the machining operation. The pull-down menus are
called by pressing the "Mach" menu in DIN/ISO mode.
Overview of the functions:
 G: Direct entry of a G code
 G menu: Pull-down menus for machining tasks
 M: Direct entry of an M function
 M menu: Pull-down menus for switching tasks
 T: Direct tool call
 F: Feed per revolution G95
 S: Cutting speed G96
 Extras, Graph.: See "Shared menu items" on page 41.

Back to the DIN/ISO main menu
HEIDENHAIN MANUALplus 620, CNC PILOT 640
199
4.2 Definition of workpiece blank
4.2 Definition of workpiece blank
Chuck part bar/tube G20-Geo
G20 defines the contour of a cylinder/hollow cylinder.
Parameters
X
 Cylinder/hollow cylinder diameter
 Diameter of circumference of a polygonal blank
Z
Length of the blank
K
Right edge (distance between workpiece zero point and right
edge)
I
Inside diameter of hollow cylinders
Beispiel: G20-Geo
...
BLANK
N1 G20 X80 Z100 K2 I30 [hollow cylinder]
...
Cast part G21-Geo
G21 generates the contour of the blank part from the contour of the
finished part—plus the equidistant oversize P.
Parameters
P
Equidistant oversize (reference: finished part contour)
Q Bore hole Y/N (default: 0)
 0: Without hole
 1: With hole
G21 cannot be used to describe an "auxiliary blank."
Beispiel: G21-Geo
...
BLANK
N1 G21 P5 Q1 [cast blank]
...
FINISHED
N2 G0 X30 Z0
N3 G1 X50 BR-2
N4 G1 Z-40
N5 G1 X65
N6 G1 Z-70
...
200
DIN Programming
4.3 Basic contour elements
4.3 Basic contour elements
Starting point of turning contour G0-Geo
G0 defines the starting point of a turning contour.
Parameters
X
Starting point of contour (diameter value)
Z
Starting point of contour
PZ Starting point of contour (polar radius)
W Starting point of contour (polar angle)
Beispiel: G0-Geo
...
FINISHED
N2 G0 X30 Z0 [starting point of contour]
N3 G1 X50 BR-2
N4 G1 Z-40
N5 G1 X65
N6 G1 Z-70
...
Machining attributes for form elements
All the basic contour elements contain the chamfer/rounding form
element (BR). You can define machining attributes for this form
element and for all the other form elements (recesses, undercuts).
Parameters
BE Special feed factor for the chamfer/rounding arc during the
finishing cycle (default: 1)
BF
BD
BP
BH
Special feed rate = active feed rate * BE
Special feed rate for the chamfer/rounding arc during the
finishing cycle (default: no special feed rate)
Additive compensation number for the chamfer/rounding arc
(901-916)
Equidistant oversize (at constant distance) for the chamfer/
rounding arc
Type of oversize for the chamfer/rounding arc
 0: Absolute oversize
 1: Additive oversize
HEIDENHAIN MANUALplus 620, CNC PILOT 640
201
4.3 Basic contour elements
Line segment in a contour G1-Geo
G1 defines a line segment in a turning contour.
Parameters
X
End point of contour element (diameter value)
Z
End point of contour element
AN Angle to rotary axis (for angle direction see graphic support
window)
Q
Point of intersection. End point if the line segment intersects a
circular arc (default: 0):
BR
 0: Near point of intersection
 1: Far point of intersection
Chamfer/rounding. Defines the transition to the next contour
element. When entering a chamfer/rounding, program the
theoretical end point.
 No input: Tangential transition
 BR=0: No tangential transition
 BR>0: Radius of rounding
 BR<0: Width of chamfer
PZ End point of contour element (polar radius; reference:
workpiece zero point)
W End point of contour element (polar angle; reference: workpiece
zero point)
AR Angle to rotary axis (AR corresponds to AN)
R
Line length (polar radius; reference: last contour point)
BE, BF, BD, BP and BH (see „Machining attributes for form
elements” on page 201)
FP Do not machine element (only necessary for TURN PLUS):
IC
KC
HC
 0: Do not machine basic element (straight line)
 1: Do not machine overlay element (e.g. chamfer or rounding)
 2: Do not machine basic/overlay element
Measuring cut oversize (measuring cut diameter)
Length of measuring cut
Measuring cut counter: Number of workpieces after which a
measurement is performed
Programming
 X, Z: Absolute, incremental, modal or "?"
 ANi: Angle to the subsequent element
 ARi: Angle to the previous element
202
DIN Programming
4.3 Basic contour elements
Example: G1-Geo
...
FINISHED
N2 G0 X0 Z0
Starting point
N3 G1 X50 BR-2
Vertical line with chamfer
N4 G1 Z-20 BR2
Horizontal line with radius
N5 G1 X70 Z-30
Oblique cut with absolute target coordinates
N6 G1 Zi-5
Horizontal line segment, incremental
N7 G1 Xi10 AN30
Incremental and angle
N8 G1 X92 Zi-5
Incremental and absolute mixed
N9 G1 X? Z-80
Calculate the X coordinate
N10 G1 X100 Z-100 AN10
End point and angle with unknown starting point
...
HEIDENHAIN MANUALplus 620, CNC PILOT 640
203
4.3 Basic contour elements
Circular arc of turning contour G2/G3-Geo
G2/G3 defines a circular arc in a contour with incremental center
dimensioning. Direction of rotation (see help graphic):
 G2: In clockwise direction
 G3: In counterclockwise direction
Parameters
X
End point of contour element (diameter value)
Z
End point of contour element
R
Radius
I
Center (distance from starting point to center as radius)
K
Center (distance from starting point to center)
Q
Point of intersection. End point if the circular arc intersects a
line segment or another circular arc (default: 0):
BR
 0: Near point of intersection
 1: Far point of intersection
Chamfer/rounding. Defines the transition to the next contour
element. When entering a chamfer/rounding, program the
theoretical end point.
 No input: Tangential transition
 BR=0: No tangential transition
 BR>0: Radius of rounding
 BR<0: Width of chamfer
BE, BF, BD, BP and BH (see „Machining attributes for form
elements” on page 201)
FP
Do not machine element (only necessary for TURN PLUS):
 0: Do not machine basic element (circle)
 1: Do not machine overlay element (e.g. chamfer or
rounding)
 2: Do not machine basic/overlay element
Programming X, Z: Absolute, incremental, modal or "?"
Example: G2-, G3-Geo
...
FINISHED
N1 G0 X0 Z-10
N2 G3 X30 Z-30 R30
Target point and radius
N3 G2 X50 Z-50 I19.8325 K-2.584
Target point and center, incremental
N4 G3 Xi10 Zi-10 R10
Target point (incremental) and radius
N5 G2 X100 Z? R20
Unknown target point coordinate
N6 G1 Xi-2.5 Zi-15
...
204
DIN Programming
4.3 Basic contour elements
Circular arc of turning contour G12/G13-Geo
G12/G13 defines a circular arc in a contour with absolute center
dimensioning. Direction of rotation (see help graphic):
 G12: In clockwise direction
 G13: In counterclockwise direction
Parameters
X
End point of contour element (diameter value)
Z
End point of contour element
I
Center (radius dimension)
K
Center
R
Radius
Q
Point of intersection. End point if the circular arc intersects a
line segment or another circular arc (default: 0):
BR
 0: Near point of intersection
 1: Far point of intersection
Chamfer/rounding. Defines the transition to the next contour
element. When entering a chamfer/rounding, program the
theoretical end point.
 No input: Tangential transition
 BR=0: No tangential transition
 BR>0: Radius of rounding
 BR<0: Width of chamfer
PZ End point of contour element (polar radius; reference:
workpiece zero point)
W
End point of contour element (polar angle; reference:
workpiece zero point)
PM Center point (polar radius; reference: workpiece zero point)
WM Center point (polar angle; reference: workpiece zero point)
AR Starting angle (tangential angle to rotary axis)
AN End angle (tangential angle to rotary axis)
BE, BF, BD, BP and BH (see „Machining attributes for form
elements” on page 201)
FP Do not machine element (only necessary for TURN PLUS):
 0: Do not machine basic element (straight line)
 1: Do not machine overlay element (e.g. chamfer or rounding)
 2: Do not machine basic/overlay element
Programming
 X, Z: Absolute, incremental, modal or "?"
 ARi: Angle to the previous element
 ANi: Angle to the subsequent element
HEIDENHAIN MANUALplus 620, CNC PILOT 640
205
4.3 Basic contour elements
Example: G12-, G13-Geo
...
FINISHED
N1 G0 X0 Z-10
...
N7 G13 Xi-15 Zi15 R20
Target point (incremental) and radius
N8 G12 X? Z? R15
Only the radius is known
N9 G13 X25 Z-30 R30 BR10 Q1
Rounding arc in transition and selection of
intersections
N10 G13 X5 Z-10 I22.3325 K-12.584
Target point and center, absolute
...
206
DIN Programming
4.4 Contour form elements
4.4 Contour form elements
Recess (standard) G22-Geo
G22 defines a recess on the previously programmed paraxial
reference element.
Parameters
X
Starting point of recess on the face (diameter)
Z
Starting point of recess on the lateral surface
I
Inside corner (diameter value)
K
 Recess on face: End point of the recess
 Recess on lateral surface: Recess base
Inside corner
Ii
 Recess on face: Recess base
 Recess on lateral surface: End point of the recess
Inside corner—incremental (pay attention to algebraic sign!)
Ki
 Recess on face: Recess width
 Recess on lateral surface: Recess depth
Inside corner—incremental (pay attention to algebraic sign!)
B
 Recess on face: Recess depth
 Recess on lateral surface: Recess width
Outside radius/chamfer at both sides of the recess (default: 0)
 B>0: Radius of rounding
 B<0: Width of chamfer
R
Inside radius in both corners of recess (default: 0)
BE, BF, BD, BP and BH (see „Machining attributes for form
elements” on page 201)
FP Do not machine element (only necessary for TURN PLUS):
 1: Do not machine recess
Program only X or Z.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
207
4.4 Contour form elements
Example: G22-Geo
FINISHED
N1 G0 X40 Z0
N2 G1 X80
N3 G22 X60 I70 Ki-5 B-1 R0.2
Recess on face, depth is incremental
N4 G1 Z-80
N5 G22 Z-20 I70 K-28 B1 R0.2
Longitudinal recess, width is absolute
N6 G22 Z-50 Ii-8 Ki-12 B0.5 R0.3
Longitudinal recess, width is incremental
N7 G1 X40
N8 G1 Z0
N9 G22 Z-38 Ii6 K-30 B0.5 R0.2
Longitudinal recess, inside
...
208
DIN Programming
4.4 Contour form elements
Recess (general) G23-Geo
G23 defines a recess on the previously programmed linear reference
element. The reference element can also be oblique.
Parameters
H Type of recess (default: 0)
X
 0: Symmetrical recess
 1: Relief turn
Center point of recess on the face (diameter)
Z
No input: Position is calculated
Center point of recess on the lateral surface
I
No input: Position is calculated
Recess depth and recess position
A
 I>0: Recess at the right of the reference element
 I<0: Recess at the left of the reference element
Recess width (without chamfer/rounding arc)
Recess diameter (diameter of recess base). Use U only if the
reference element runs parallel to the Z axis
Recess angle (default: 0)
B
 H=0: Angle between recess edges (0° <= A < 180°)
 H=1: Angle between reference line and recess edge (0° < A
<= 90°)
Outside radius/chamfer at corner near the starting point (default: 0)
K
U
P
 B>0: Radius of rounding
 B<0: Width of chamfer
Outside radius/chamfer at corner far from the starting point
(default: 0)
 P>0: Radius of rounding
 P<0: Width of chamfer
R
Inside radius in both corners of recess (default: 0)
BE, BF, BD, BP and BH (see „Machining attributes for form
elements” on page 201)
FP Do not machine element (only necessary for TURN PLUS):
 1: Do not machine recess
The Steuerung refers the recess depth to the reference
element. The recess base runs parallel to the reference
element.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
209
4.4 Contour form elements
Example: G23-Geo
...
FINISHED
N1 G0 X40 Z0
N2 G1 X80
N3 G23 H0 X60 I-5 K10 A20 B-1 P1 R0.2
Recess on face, depth is incremental
N4 G1 Z-40
N5 G23 H1 Z-15 K12 U70 A60 B1 P-1 R0.2
Longitudinal recess, width is absolute
N6 G1 Z-80 A45
N7 G23 H1 X120 Z-60 I-5 K16 A45 B1 P-2 R0.4
Longitudinal recess, width is incremental
N8 G1 X40
N9 G1 Z0
N10 G23 H0 Z-38 I-6 K12 A37.5 B-0.5 R0.2
Longitudinal recess, inside
...
210
DIN Programming
4.4 Contour form elements
Thread with undercut G24-Geo
G24 defines a linear basic element with a longitudinal thread and
subsequent thread undercut (DIN 76). The thread is an outside or
inside thread (metric ISO fine-pitch thread DIN 13 Part 2, Series 1).
Parameters
F
Thread pitch
I
Undercut depth (radius)
K
Width of undercut
Z
End point of the undercut
BE, BF, BD, BP and BH (see „Machining attributes for form
elements” on page 201)
FP Do not machine element (only necessary for TURN PLUS):
 1: Do not machine the element
 Program G24 only in closed contours.
 The thread is machined with G31.
Example: G24-Geo
...
FINISHED
N1 G0 X40 Z0
N2 G1 X40 BR-1.5
Starting point for thread
N3 G24 F2 I1.5 K6 Z-30
Thread with undercut
N4 G1 X50
Next transverse element
N5 G1 Z-40
...
HEIDENHAIN MANUALplus 620, CNC PILOT 640
211
4.4 Contour form elements
Undercut contour G25-Geo
G25 generates the undercut contours listed below. The undercuts are
only possible in inside contour corners in which the transverse
element is parallel to the X axis. Program G25 after the first element.
You specify the undercut type in parameter H.
Undercut type U (H=4)
Parameters
H Undercut type U: H=4
I
Undercut depth (radius)
K
Width of undercut
R
Inside radius in both corners of recess (default: 0)
P
Outside radius/chamfer (default: 0)
 P>0: Radius of rounding
 P<0: Width of chamfer
BE, BF, BD, BP and BH (see „Machining attributes for form
elements” on page 201)
FP Do not machine element (only necessary for TURN PLUS):
 1: Do not machine undercut
Beispiel: Call G25-Geo type U
...
N.. G1 Z-15
[longitudinal element]
N.. G25 H4 I2 K4 R0.4 P-0.5 [type U]
N.. G1 X20
[transverse element]
...
212
DIN Programming
4.4 Contour form elements
Undercut DIN 509 E (H=0.5)
Parameters
H Undercut type DIN 509 E: H=0 or H=5
I
Undercut depth (radius)
K
Width of undercut
R
Undercut radius (in both corners of the undercut)
W Undercut angle
BE, BF, BD, BP and BH (see „Machining attributes for form
elements” on page 201)
The Steuerung uses the diameter to calculate the parameters that you
do not define.
Beispiel: Call G25-Geo DIN 509 E
...
N.. G1 Z-15
[longitudinal element]
N.. G25 H5
[DIN 509 E]
N.. G1 X20
[transverse element]
...
Undercut DIN 509 F (H=6)
Parameters
H Undercut type DIN 509 F: H=6
I
Undercut depth (radius)
K
Width of undercut
R
Undercut radius (in both corners of the undercut)
P
Face depth
W Undercut angle
A
Transverse angle
BE, BF, BD, BP and BH (see „Machining attributes for form
elements” on page 201)
The Steuerung uses the diameter to calculate the parameters that you
do not define.
Beispiel: Call G25-Geo DIN 509 F
...
N.. G1 Z-15
[longitudinal element]
N.. G25 H6
[DIN 509 F]
N.. G1 X20
[transverse element]
...
HEIDENHAIN MANUALplus 620, CNC PILOT 640
213
4.4 Contour form elements
Undercut DIN 76 (H=7)
Program only FP. All the other values are automatically calculated from
the thread pitch in the standard table if they are not defined.
Parameters
H Undercut type DIN 76: H=7
I
Undercut depth (radius)
K
Width of undercut
R
Undercut radius in both corners of the undercut (default:
R=0.6*I)
W Undercut angle (default: 30°)
FP Thread pitch
BE, BF, BD, BP and BH (see „Machining attributes for form
elements” on page 201)
Beispiel: Call G25-Geo DIN 76
...
N.. G1 Z-15
[longitudinal element]
N.. G25 H7 FP2 [DIN 76]
N.. G1 X20
[transverse element]
...
Undercut type H (H=8)
If you do not enter W, the angle will be calculated on the basis of K and
R. The end point of the undercut is then located at the "contour
corner."
Parameters
H Undercut type H: H=8
K
Width of undercut
R
Undercut radius—no input: The circular element is not machined
W Plunge angle—no input: W is calculated
BE, BF, BD, BP and BH (see „Machining attributes for form
elements” on page 201)
Beispiel: Call G25-Geo type H
...
N.. G1 Z-15
[longitudinal element]
N.. G25 H8 K4 R1 W30 [type H]
N.. G1 X20
[transverse element]
...
214
DIN Programming
4.4 Contour form elements
Undercut type K (H=9)
Parameters
H Undercut type K: H=9
I
Undercut depth
R
Undercut radius—no input: The circular element is not machined
W Undercut angle
A
Angle to longitudinal axis (default: 45°)
BE, BF, BD, BP and BH (see „Machining attributes for form
elements” on page 201)
Beispiel: Call G25-Geo type K
...
N.. G1 Z-15
[longitudinal element]
N.. G25 H9 I1 R0.8 W40 [type K]
N.. G1 X20
[transverse element]
...
HEIDENHAIN MANUALplus 620, CNC PILOT 640
215
4.4 Contour form elements
Thread (standard) G34-Geo
G34 defines a simple or concatenated external or internal thread
(metric ISO fine-pitch thread DIN 13 Series 1). The Steuerung
calculates all the required values.
Parameters
F
Thread pitch (default: pitch from the standard table)
Threads are concatenated by programming several G1/G34 blocks
after each other.
 You need to program a linear contour element as a
reference before G34 or in the NC block containing G34.
 Machine the thread with G31.
Beispiel: G34
...
FINISHED
N1 G0 X0 Z0
N2 G1 X20 BR-2
N3 G1 Z-30
N4 G34 [metric ISO]
N5 G25 H7 I1.7 K7
N6 G1 X30 BR-1.5
N7 G1 Z-40
N8 G34 F1.5 [metric ISO fine-pitch thread]
N9 G25 H7 I1.5 K4
N10 G1 X40
N11 G1 Z-60
...
216
DIN Programming
4.4 Contour form elements
Thread (general) G37-Geo
G37 defines the different types of thread. Multi-start threads and
concatenated threads are possible. Threads are concatenated by
programming several G01/G37 blocks after each other.
Parameters
Q Type of thread (default: 1)
F
 1: Metric ISO fine-pitch thread (DIN 13 Part 2, Series 1)
 2: Metric ISO thread (DIN 13 Part 1, Series 1)
 3: Metric ISO tapered thread (DIN 158)
 4: Metric ISO tapered fine-pitch thread (DIN 158)
 5: Metric ISO trapezoid thread (DIN 103 Part 2, Series 1)
 6: Flat metric trapezoid thread (DIN 380 Part 2, Series 1)
 7: Metric buttress thread (DIN 513 Part 2, Series 1)
 8: Cylindrical round thread (DIN 405 Part 1, Series 1)
 9: Cylindrical Whitworth thread (DIN 11)
 10: Tapered Whitworth thread (DIN 2999)
 11: Whitworth pipe thread (DIN 259)
 12: Nonstandard thread
 13: UNC US coarse thread
 14: UNF US fine-pitch thread
 15: UNEF US extra-fine-pitch thread
 16: NPT US taper pipe thread
 17: NPTF US taper dryseal pipe thread
 18: NPSC US cylindrical pipe thread with lubricant
 19: NPFS US cylindrical pipe thread without lubricant
Thread pitch
P
K
D
 Required for Q=1, 3 to 7, 12.
 For other thread types, F is calculated from the diameter if it
was not programmed.
Thread depth—enter only for Q=12
Run-out length for threads without undercut (default: 0)
Reference point (default: 0)
H
A
W
R
E
 0: Runout of thread at the end of the reference element
 1: Runout of thread at the beginning of the reference element
Number of thread turns (default: 1)
Thread angle at left—enter only for Q=12
Thread angle at right—enter only for Q=12
Thread width—enter only for Q=12
Variable pitch (default: 0)
V
Increase/decrease the pitch per revolution by E.
Direction of thread
 0: Right-hand thread
 1: Left-hand thread
Beispiel: G37
...
FINISHED
N1 G0 X0 Z0
N2 G1 X20 BR-2
N3 G1 Z-30
N4 G37 Q2 [metric ISO]
N5 G25 H7 I1.7 K7
N6 G1 X30 BR-1.5
N7 G1 Z-40
N8 G37 F1.5 [metric ISO fine-pitch thread]
N9 G25 H7 FP1.5
N10 G1 X40
N11 G1 Z-60
...
HEIDENHAIN MANUALplus 620, CNC PILOT 640
217
4.4 Contour form elements
Beispiel: G37 Concatenated
 Before G37, program a linear contour element as a
reference.
 Machine the thread with G31.
 For standard threads, the parameters P, R, A and W are
defined by the Steuerung.
 Use Q=12 if you wish to use individual parameters.
...
AUXILIARY CONTOUR ID"G37_Concatenated"
N37 G0 X0 Z0
N 38 G1 X20
N 39 G1 Z-30
N 40 G37 F2 [metric ISO]
Danger of collision!
The thread is generated to the length of the reference
element. Another linear element without undercut is to be
programmed as overrun.
N 41 G1 X30 Z-40
N 42 G37 Q2
N 43 G1 Z-70
N 44 G37 F2
...
218
DIN Programming
4.4 Contour form elements
Bore hole (centric) G49-Geo
G49 defines a single hole with countersink and thread at the turning
center (front or rear face). The G49 hole is a form element, not part of
the contour.
Parameters
Z
Starting position for hole (reference point)
B
Hole diameter
P
Depth of hole (excluding point)
W Point angle (default: 180°)
R
Sinking diameter
U Sinking depth
E
Sinking angle
I
Thread diameter
J
Thread depth
K
Thread chamfer
F
Thread pitch
V
Left-hand or right-hand thread (default: 0)
A
 0: Right-hand thread
 1: Left-hand thread
Angle corresponding to the position of the hole (default: 0)
O
 A=0°: Front face
 A=180°: Rear face
Centering diameter
 Program G49 in the FINISHED section, not in AUXILIARY
CONTOUR, FACE or REAR.
 Machine the G49 hole with G71...G74.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
219
4.5 Attributes for contour description
4.5 Attributes for contour
description
Overview of attributes for contour description
G38
Special feed factor for basic elements and
form elements—modal
Page 220
G52
Equidistant oversize for basic elements and
form elements—modal
Page 222
G95
Finishing feed rate for basic elements and
form elements—modal
Page 223
G149 Additive compensation for basic elements and
form elements—modal
Page 223
 Once programmed, G38-, G52-, G95- and G149-Geo
remain in effect for all contour elements until the
function is programmed again without defining
parameters.
 For form elements, you can program different attributes
directly in the definition of the form element (see
„Machining attributes for form elements” on page 201).
 The attributes for contour description influence the
finishing feed rate of the Cycles G869 and G890, not the
finishing feed rate in recessing cycles.
Feed rate reduction G38-Geo
G38 activates the special feed rate for the finishing cycle G890. The
special feed rate applies to basic contour elements and form
elements. It is a modal function.
Parameters
E
Special feed factor (default: 1)
Special feed rate = active feed rate * E
 G38 is a modal function.
 Program G38 before the contour element for which it is
intended.
 G38 replaces a special feed rate.
 To cancel the special feed factor, program G38 without
parameters.
220
DIN Programming
4.5 Attributes for contour description
Attributes for superimposed elements G39-Geo
G39 influences the finishing feed rate of G890 with the form
elements:
 Chamfers/rounding arcs (for connecting basic elements)
 Undercuts
 Recesses
Affected machining: Special feed rate, surface roughness, additive D
compensation, equidistant oversizes.
Parameters
F
Feed per revolution
V
Type of surface roughness (see also DIN 4768)
RH
D
P
H
 1: General surface roughness (profile depth) Rt1
 2: Surface roughness Ra
 3: Surface roughness Rz
Surface roughness [µm, inch mode: µinch]
Number of the additive compensation (901 <= D <= 916)
Oversize (radius)
P applies as an absolute or additive value (default: 0)
E
 0: P replaces G57/G58 oversizes
 1: P is added to G57/G58 oversizes
Special feed factor (default: 1)
Special feed rate = active feed rate * E
 Use surface roughness (V, RH), finishing feed rate (F)
and special feed rate ("E") alternately!
 G39 is a non-modal function.
 Program G39 before the contour element for which it is
intended.
 G50 preceding a cycle (MACHINING section) cancels a
finishing oversize programmed for that cycle with G39.
Function G39 can be replaced by directly entering the
attributes in the contour elements dialog. The function is
necessary to execute imported programs correctly.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
221
4.5 Attributes for contour description
Separation point G44
During automatic program creation with TURN PLUS, you can define
the separation point for rechucking with function G44.
Parameters
D
Location of separation point:
 0: Start of the basic element as separation point
 1: Target of the basic element as separation point
If no separation point was defined, TURNplus uses the
largest diameter as separation point for outside machining
and the smallest diameter as separation point for inside
machining.
Oversize G52-Geo
G52 defines an equidistant oversize that applies to basic contour
elements and form elements and is taken into consideration in G810,
G820, G830, G860 and G890.
Parameters
P
Oversize (radius)
H
P applies as an absolute or additive value (default: 0)
 0: P replaces G57/G58 oversizes
 1: P is added to G57/G58 oversizes
 G52 is a modal function.
 Program G52 in the NC block for which it is intended.
 G50 preceding a cycle (MACHINING section) cancels an
oversize programmed for that cycle with G52.
222
DIN Programming
G95 influences the finishing feed rate of G890 for basic contour
elements and form elements.
Parameters
F
Feed per revolution
 The G95 finishing feed rate replaces a finishing feed rate
defined in the machining section.
 G95 is a modal function.
 To cancel a finishing feed rate set with G95, program
G95 without an input value.
Beispiel: Attributes in contour description G95
...
FINISHED
N1 G0 X0 Z0
N2 G1 X20 BR-1
N3 G1 Z-20
N4 G25 H5 I0.3 K2.5 R0.6 W15
N5 G1 X40 BR-1
N6 G95 F0.08
N7 G1 Z-40
N8 G25 H5 I0.3 K2.5 R0.6 W15 BF0
N9 G95
N10 G1 X58 BR-1
N11 G1 Z-60
...
Additive compensation G149-Geo
G149 followed by a D number activates/deactivates an additive
compensation function. The Steuerung manages the 16 toolindependent compensation values in an internal table. The
compensation values are managed in the Program Run mode (see
"Program Run mode" in the User's Manual).
Parameters
D
Additive compensation (default: D900)
 D=900: Deactivates the additive compensation
 D=901 to 916: Activates the additive compensation D
 Note the direction of contour description.
 Additive compensation is effective from the block in
which G149 is programmed.
 Additive compensation remains in effect up to:
 the next G149 D900,
 up to the end of the finished part description.
Beispiel: Attributes in contour description G149
...
FINISHED
N1 G0 X0 Z0
N2 G1 X20 BR-1
N3 G1 Z-20
N4 G25 H5 I0.3 K2.5 R0.6 W15
N5 G1 X40 BR-1
N6 G149 D901
N7 G1 Z-40
N8 G25 H5 I0.3 K2.5 R0.6 W15 BD900
N9 G149 D900
N10 G1 X58 BR-1
N 12 G1 Z-60
...
HEIDENHAIN MANUALplus 620, CNC PILOT 640
223
4.5 Attributes for contour description
Feed per revolution G95-Geo
4.6 C-axis contours—Fundamentals
4.6 C-axis contours—
Fundamentals
Milling contour position
Define the reference plane or the reference diameter in the section
code. Specify the depth and position of a milling contour (pocket,
island) in the contour definition:
 With depth P programmed in the previous G308 cycle.
 Alternatively on figures: Cycle parameter depth P.
The algebraic sign of "P" defines the position of the milling contour:
 P<0: Pocket
 P>0: Island
Position of milling contour
Section
P
Surface
Milling floor
FACE_C
P<0
Z
Z+P
P>0
Z+P
Z
P<0
Z
Z–P
P>0
Z–P
Z
P<0
X
X+(P*2)
P>0
X+(P*2)
X
REAR_C
LATERAL_C
 X: Reference diameter from the section code
 Z: Reference plane from the section code
 P: Depth from G308 or from cycle parameter
The area milling cycles mill the surface specified in the
contour definition. Islands within this surface are not
taken into consideration.
Contours in more than one plane (hierarchically nested contours):
 A plane begins with G308 and ends with G309.
 G308 defines a new reference plane/reference diameter. The first
G308 uses the reference plane defined in the section code. Each
following G308 defines a new plane. Calculation:
New reference plane = Reference plane + P (from previous G308).
 G309 switches back to the previous reference plane.
224
DIN Programming
4.6 C-axis contours—Fundamentals
Beginning of pocket/island G308-Geo
G308 defines a new reference plane / reference diameter in
hierarchically nested contours.
Parameters
P
Depth for pockets, height for islands
ID
Name of the contour for reference from units or cycles
HC Milling/drilling attribute:
Q
 1: Contour milling
 2: Pocket milling
 3: Area milling
 4: Deburring
 5: Engraving
 6: Contour milling and deburring
 7: Pocket milling and deburring
 14: Do not machine
Milling location:
H
 0: On the contour
 1: Inside/left
 2: Outside/right
Direction:
D
I
W
BR
RB
 0: Up-cut milling
 1: Climb milling
Cutter diameter
Limit diameter
Angle of the chamfer
Chamfer width
Retraction plane
End of pocket/island G309-Geo
G309 defines the end of a reference plane. Every reference plane
defined with G308 must be ended with G309 (See "Milling contour
position" on page 224.).
HEIDENHAIN MANUALplus 620, CNC PILOT 640
225
4.6 C-axis contours—Fundamentals
Example of G308/G309
...
FINISHED
...
FACE_C Z0
Define reference plane
N7 G308 P-5 ID"Rectangle"
Beginning of rectangle with depth of –5
N8 G305 XK-5 YK-10 K50 B30 R3 A0
Rectangle
N9 G308 P-10 ID"Circle"
Beginning of "full circle in rectangle" with depth –10
N10 G304 XK-3 YK-5 R8
Full circle
N11 G309
End of full circle
N12 G309
End of rectangle
LATERAL_C X100
Define reference diameter
N13 G311 Z-10 C45 A0 K18 B8 P-5
Linear slot with depth –5
...
226
DIN Programming
4.6 C-axis contours—Fundamentals
Circular pattern with circular slots
For circular slots in circular patterns you program the pattern positions,
the center of curvature, the curvature radius and the position of the
slots.
The Steuerung positions the slots as follows:
 Slots are arranged at the distance of the pattern radius about the
pattern center if
 Pattern center = center of curvature and
 Pattern radius = curvature radius
 Slots are arranged at the distance of the pattern radius + curvature
radius about the pattern center if
 Pattern center <> center of curvature or
 Pattern radius <> curvature radius
In addition, the position influences the arrangement of the slots:
 Normal position: The starting angle of the slot applies as a relative
value to the pattern position. The starting angle is added to the
pattern position.
 Original position: The starting angle of the slot applies as an
absolute value.
The following examples show the programming of a circular pattern
with circular slots:
HEIDENHAIN MANUALplus 620, CNC PILOT 640
227
4.6 C-axis contours—Fundamentals
Slot centerline as reference and normal position
Programming:
 Pattern center = center of curvature
 Pattern radius = curvature radius
 Normal position
These commands arrange the slots at the distance of the pattern
radius about the pattern center.
Example: Slot centerline as reference, normal position
N.. G402 Q4 K30 A0 XK0 YK0 H0
Circular pattern, normal position
N.. G303 I0 J0 R15 A-20 W20 B3 P1
Circular slot
Slot centerline as reference and original position
Programming:
 Pattern center = center of curvature
 Pattern radius = curvature radius
 Original position
These commands arrange all slot at the same position.
Example: Slot centerline as reference, original position
N.. G402 Q4 K30 A0 XK0 YK0 H1
Circular pattern, original position
N.. G303 I0 J0 R15 A-20 W20 B3 P1
Circular slot
228
DIN Programming
4.6 C-axis contours—Fundamentals
Center of curvature as reference and normal position
Programming:
 Pattern center <> center of curvature
 Pattern radius = curvature radius
 Normal position
These commands arrange the slots at the distance of the pattern
radius plus curvature radius about the pattern center.
Example: Center of curvature as reference, normal position
N.. G402 Q4 K30 A0 XK5 YK5 H0
Circular pattern, normal position
N.. G303 I0 J0 R15 A-20 W20 B3 P1
Circular slot
Center of curvature as reference and original position
Programming:
 Pattern center <> center of curvature
 Pattern radius = curvature radius
 Original position
These commands arrange the slots at the distance of the pattern
radius plus curvature radius about the pattern center while keeping the
starting and ending angle.
Example: Center of curvature as reference, original position
N.. G402 Q4 K30 A0 XK5 YK5 H1
Circular pattern, original position
N.. G303 I0 J0 R15 A-20 W20 B3 P1
Circular slot
HEIDENHAIN MANUALplus 620, CNC PILOT 640
229
4.7 Front and rear face contours
4.7 Front and rear face contours
Starting point of front/rear face contour
G100-Geo
G100 defines the starting point of a front or rear face contour.
Parameters
X
Starting point in polar coordinates (diameter)
C
Starting point in polar coordinates (angular dimension)
XK Starting point in Cartesian coordinates
YK Starting point in Cartesian coordinates
230
DIN Programming
4.7 Front and rear face contours
Line segment in front/rear face contour G101Geo
G101 defines a line segment in a contour on the front face/rear face.
Parameters
X
End point in polar coordinates (diameter)
C
End point in polar coordinates (angular dimension)
XK End point in Cartesian coordinates
YK End point in Cartesian coordinates
AN Angle to positive XK axis
Q
Point of intersection. End point if the line segment intersects a
circular arc (default: 0):
BR
AR
R
 0: Near point of intersection
 1: Far point of intersection
Chamfer/rounding. Defines the transition to the next contour
element. When entering a chamfer/rounding, program the
theoretical end point.
 No input: Tangential transition
 BR=0: No tangential transition
 BR>0: Radius of rounding
 BR<0: Width of chamfer
Angle to positive XK axis (AR corresponds to AN)
Length (polar radius; reference: last contour point)
Programming
 X, XK, YX: Absolute, incremental, modal or "?"
 C: Absolute, incremental or modal
 ARi: Angle to the previous element
 ANi: Angle to the subsequent element
HEIDENHAIN MANUALplus 620, CNC PILOT 640
231
4.7 Front and rear face contours
Circular arc in front/rear face contour G102/
G103-Geo
G102/G103 defines a circular arc in a front or rear face contour.
Direction of rotation (see help graphic):
 G102: In clockwise direction
 G103: In counterclockwise direction
Parameters
X
End point in polar coordinates (diameter)
C
End point in polar coordinates (angular dimension)
XK End point in Cartesian coordinates
YK End point in Cartesian coordinates
R
Radius
I
Center in Cartesian coordinates
J
Center in Cartesian coordinates
Q
Point of intersection. End point if the circular arc intersects a line
segment or another circular arc (default: 0):
BR
 0: Near point of intersection
 1: Far point of intersection
Chamfer/rounding. Defines the transition to the next contour
element. When entering a chamfer/rounding, program the
theoretical end point.
 No input: Tangential transition
 BR=0: No tangential transition
 BR>0: Radius of rounding
 BR<0: Width of chamfer
XM Center point (polar radius; reference: workpiece zero point)
CM Center point (polar angle; reference: workpiece zero point)
AR Starting angle (tangential angle to rotary axis)
AN End angle (tangential angle to rotary axis)
Programming
 X, XK, YX: Absolute, incremental, modal or "?"
 C: Absolute, incremental or modal
 I, J: Absolute or incremental
 XM, CM: Absolute or incremental
 ARi: Angle to the previous element
 ANi: Angle to the subsequent element
 End point must not be the starting point (no full circle).
232
DIN Programming
4.7 Front and rear face contours
Bore hole on front/rear face G300-Geo
G300 defines a hole with countersinking and thread in a front or rear
face contour.
Parameters
XK Center in Cartesian coordinates
YK Center in Cartesian coordinates
B
Hole diameter
P
Depth of hole (excluding point)
W Point angle (default: 180°)
R
Sinking diameter
U Sinking depth
E
Sinking angle
I
Thread diameter
J
Thread depth
K
Thread runout length
F
Thread pitch
V
Left-hand or right-hand thread (default: 0)
A
 0: Right-hand thread
 1: Left-hand thread
Angle to Z axis; angle of the hole
O
 Range for front face: –90° < A < 90° (default: 0°)
 Range for rear face: 90° < A < 270° (default: 180°)
Centering diameter
Machine the G300 holes with G71...G74.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
233
4.7 Front and rear face contours
Linear slot on front/rear face G301-Geo
G301 defines a linear slot in a contour on the front or rear face.
Parameters
XK Center in Cartesian coordinates
YK Center in Cartesian coordinates
X
Diameter (center point in polar coordinates)
C
Angle (center point in polar coordinates)
A
Angle to XK axis (default: 0°)
K
Slot length
B
Slot width
P
Depth/height (default: "P" from G308)
 P<0: Pocket
 P>0: Island
Circular slot on front/rear face G302/G303-Geo
G302/G303 defines a circular slot in a contour on the front face/rear
face.
 G302: Circular slot clockwise
 G303: Circular slot counterclockwise
Parameters
I
Center of curvature in Cartesian coordinates
J
Center of curvature in Cartesian coordinates
X
Diameter (center point in polar coordinates)
C
Angle (center point in polar coordinates)
R
Curvature radius (reference: center point path of the slot)
A
Starting angle; reference: XK axis (default: 0°)
W End angle; reference: XK axis (default: 0°)
B
Slot width
P
Depth/height (default: "P" from G308)
 P<0: Pocket
 P>0: Island
234
DIN Programming
4.7 Front and rear face contours
Full circle on front/rear face G304-Geo
G304 defines a full circle in a contour on the front face/rear face.
Parameters
XK Center in Cartesian coordinates
YK Center in Cartesian coordinates
X
Diameter (center point in polar coordinates)
C
Angle (center point in polar coordinates)
R
Radius
P
Depth/height (default: "P" from G308)
 P<0: Pocket
 P>0: Island
Rectangle on front/rear face G305-Geo
G305 defines a rectangle in a contour on the front face/rear face.
Parameters
XK Center in Cartesian coordinates
YK Center in Cartesian coordinates
X
Diameter (center point in polar coordinates)
C
Angle (center point in polar coordinates)
A
Angle to XK axis (default: 0°)
K
Length
B
(Height) width
R
Chamfer/rounding (default: 0°)
P
 R>0: Radius of rounding
 R<0: Width of chamfer
Depth/height (default: "P" from G308)
 P<0: Pocket
 P>0: Island
HEIDENHAIN MANUALplus 620, CNC PILOT 640
235
4.7 Front and rear face contours
Eccentric polygon on front/rear face G307-Geo
G307 defines a polygon in a contour on the front face/rear face.
Parameters
XK Center in Cartesian coordinates
YK Center in Cartesian coordinates
X
Diameter (center point in polar coordinates)
C
Angle (center point in polar coordinates)
A
Angle of a polygon edge to XK axis (default: 0°)
Q Number of edges (Q > 2)
K
Edge length
R
 K>0: Edge length
 K<0: Inscribed circle diameter
Chamfer/rounding (default: 0°)
P
 R>0: Radius of rounding
 R<0: Width of chamfer
Depth/height (default: "P" from G308)
 P<0: Pocket
 P>0: Island
236
DIN Programming
4.7 Front and rear face contours
Linear pattern on front/rear face G401-Geo
G401 defines a linear hole pattern or figure pattern on the front or rear
face. G401 is effective for the hole/figure defined in the following
block (G300 to 305, G307).
Parameters
Q Number of figures (default: 1)
XK Starting point in Cartesian coordinates
YK Starting point in Cartesian coordinates
I
End point in Cartesian coordinates
J
End point in Cartesian coordinates
Ii
Distance (XKi) between figures (pattern distance)
Ji Distance (YKi) between figures (pattern distance)
A
Angle of longitudinal axis to XK axis (default: 0°)
R
Total length of pattern
Ri Distance between figures (pattern distance)
 Program the hole/figure in the following block without a
center.
 The milling cycle (MACHINING section) calls the hole/
figure in the following block—not the pattern definition.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
237
4.7 Front and rear face contours
Circular pattern on front/rear face G402-Geo
G402 defines a circular hole pattern or figure pattern on the front or
rear face. G402 is effective for the hole/figure defined in the following
block (G300 to 305, G307).
Parameters
Q Number of figures
K
Pattern diameter
A
Starting angle—position of the first figure; reference: XK axis
(default: 0°)
W End angle—position of the last figure; reference: XK axis
(default: 360°)
Wi Angle between figures
V
Direction—orientation (default: 0)
 V=0, without W: Figures are arranged on a full circle
 V=0, with W: Figures are arranged on the longer circular arc
 V=0, with Wi: The algebraic sign of Wi defines the direction
(Wi<0: clockwise)
 V=1, with W: Clockwise
 V=1, with Wi: Clockwise (algebraic sign of Wi has no effect)
 V=2, with W: Counterclockwise
 V=2, with Wi: Counterclockwise (algebraic sign of Wi has no
effect)
XK Center in Cartesian coordinates
YK Center in Cartesian coordinates
H Position of the figures (default: 0)
 H=0: Normal position—the figures are rotated about the circle
center (rotation)
 H=1: Original position—the position of the figures relative to
the coordinate system remains unchanged (translation)
 Program the hole/figure in the following block without a
center. Exception: circular slot: See "Circular pattern
with circular slots" on page 227..
 The milling cycle (MACHINING section) calls the hole/
figure in the following block—not the pattern definition.
238
DIN Programming
4.8 Lateral surface contours
4.8 Lateral surface contours
Starting point of lateral surface contour
G110-Geo
G110 defines the starting point of a lateral-surface contour.
Parameters
Z
Starting point
C
Starting point (starting angle or polar angle)
CY Starting point as linear value; reference: unrolled reference
diameter
PZ Starting point (polar radius)
Program either Z, C or Z, CY.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
239
4.8 Lateral surface contours
Line segment in a lateral surface contour
G111-Geo
G111 defines a line segment in a lateral-surface contour.
Parameters
Z
End point
C
End point (end angle or polar angle)
CY End point as linear value; reference: unrolled reference
diameter
AN Angle to Z axis
Q
Point of intersection. End point if the line segment intersects a
line (default: 0):
BR
PZ
AR
R
 Q=0: Near point of intersection
 Q=1: Far point of intersection
Chamfer/rounding. Defines the transition to the next contour
element. When entering a chamfer/rounding, program the
theoretical end point.
 No input: Tangential transition
 BR=0: No tangential transition
 BR>0: Radius of rounding
 BR<0: Width of chamfer
End point (polar radius)
Angle to Z axis (AR corresponds to AN)
Length (polar radius; reference: last contour point)
Programming
 Z, CY: Absolute, incremental, modal or "?"
 C: Absolute, incremental or modal
 ARi: Angle to the previous element
 ANi: Angle to the subsequent element
 Program either Z, C or Z, CY.
240
DIN Programming
4.8 Lateral surface contours
Circular arc in lateral surface contour G112/
G113-Geo
G112/G113 defines a circular arc in a lateral-surface contour. Direction
of rotation: See help graphic
Parameters
Z
End point
C
End point (end angle or polar angle)
CY End point as linear value; reference: unrolled reference
diameter
R
Radius
K
Center point in Z direction
J
Angle of the center point as a linear value
Q
Point of intersection. End point if the circular arc intersects a line
segment or another circular arc (default: 0):
BR
 0: Near point of intersection
 1: Far point of intersection
Chamfer/rounding. Defines the transition to the next contour
element. When entering a chamfer/rounding, program the
theoretical end point.
 No input: Tangential transition
 BR=0: No tangential transition
 BR>0: Radius of rounding
 BR<0: Width of chamfer
PZ End point (polar radius)
W Center point (polar angle; reference: workpiece zero point)
PM Center point (polar radius; reference: workpiece zero point)
AR Starting angle (tangential angle to rotary axis)
AN End angle (tangential angle to rotary axis)
Programming
 Z, CY: Absolute, incremental, modal or "?"
 C: Absolute, incremental or modal
 K, J: Absolute or incremental
 PZ, W, PM: Absolute or incremental
 ARi: Angle to the previous element
 ANi: Angle to the subsequent element
 Program either Z and C or Z and CY, and either K and W
or K and J
 Program either center or radius
 For radius: Only arcs <= 180° are possible
HEIDENHAIN MANUALplus 620, CNC PILOT 640
241
4.8 Lateral surface contours
Hole on lateral surface G310-Geo
G310 defines a hole with countersink and thread in a lateral surface
contour.
Parameters
Z
Center (Z position)
CY Center as linear value; reference: unrolled reference diameter
C
Center (angle)
B
Hole diameter
P
Depth of hole (excluding point)
W Point angle (default: 180°)
R
Sinking diameter
U Sinking depth
E
Sinking angle
I
Thread diameter
J
Thread depth
K
Thread runout length
F
Thread pitch
V
Left-hand or right-hand thread (default: 0)
A
O
 V=0: Right-hand thread
 V=1: Left-hand thread
Angle to Z axis; range: 0° < A < 180°; (default: 90° = vertical
hole)
Centering diameter
Machine the G310 holes with G71...G74.
242
DIN Programming
4.8 Lateral surface contours
Linear slot on lateral surface G311-Geo
G311 defines a linear slot in a lateral-surface contour.
Parameters
Z
Center (Z position)
CY Center as linear value; reference: unrolled reference diameter
C
Center (angle)
A
Angle to Z axis (default: 0°)
K
Slot length
B
Slot width
P
Pocket depth (default: "P" from G308)
Circular slot on lateral surface G312/G313-Geo
G312/G313 defines a circular slot in a lateral-surface contour.
 G312: Circular slot clockwise
 G313: Circular slot counterclockwise
Parameters
Z
Center
CY Center as linear value; reference: unrolled reference diameter
C
Center (angle)
R
Radius; reference: center point path of the slot
A
Starting angle; reference: Z axis (default: 0°)
W End angle; reference: Z axis
B
Slot width
P
Pocket depth (default: "P" from G308)
HEIDENHAIN MANUALplus 620, CNC PILOT 640
243
4.8 Lateral surface contours
Full circle on lateral surface G314-Geo
G314 defines a full circle in a lateral-surface contour.
Parameters
Z
Center
CY Center as linear value; reference: unrolled reference diameter
C
Center (angle)
R
Radius
P
Pocket depth (default: "P" from G308)
Rectangle on lateral surface G315-Geo
G315 defines a rectangle in a lateral-surface contour.
Parameters
Z
Center
CY Center as linear value; reference: unrolled reference diameter
C
Center (angle)
A
Angle to Z axis (default: 0°)
K
Length
B
Width
R
Chamfer/rounding (default: 0°)
P
244
 R>0: Radius of rounding
 R<0: Width of chamfer
Pocket depth (default: "P" from G308)
DIN Programming
4.8 Lateral surface contours
Eccentric polygon on lateral surface G317-Geo
G317 defines a polygon in a lateral-surface contour.
Parameters
Z
Center
CY Center as linear value; reference: unrolled reference diameter
C
Center (angle)
Q Number of edges (Q > 2)
A
Angle to Z axis (default: 0°)
K
Edge length
R
 K>0: Edge length
 K<0: Inscribed circle diameter
Chamfer/rounding (default: 0°)
P
 R>0: Radius of rounding
 R<0: Width of chamfer
Pocket depth (default: "P" from G308)
HEIDENHAIN MANUALplus 620, CNC PILOT 640
245
4.8 Lateral surface contours
Linear pattern on lateral surface G411-Geo
G411 defines a linear hole or figure pattern on the lateral surface. G411
is effective for the hole/figure defined in the following block (G310 to
315, G317).
Parameters
Q
Number of figures (default: 1)
Z
Starting point
C
Starting point (starting angle)
CY Starting point as linear value; reference: unrolled reference
diameter
ZE End point
ZEi Distance between figures in Z direction
W
End point (end angle)
Wi Angular distance between figures
A
Angle to Z axis; (default: 0°)
R
Total length of pattern
Ri
Distance between figures (pattern distance)
 If you program Q, Z and C, the holes/figures are
arranged at a regular spacing on the lateral surface.
 Program the hole/figure in the following block without a
center.
 The milling cycle calls the hole/figure in the following
block—not the pattern definition.
246
DIN Programming
4.8 Lateral surface contours
Circular pattern on lateral surface G412-Geo
G412 defines a circular hole or figure pattern on the lateral surface.
G412 is effective for the hole/figure defined in the following block
(G310 to 315, G317).
Parameters
Q Number of figures
K
Pattern diameter
A
Starting angle—position of the first figure; reference: Z axis;
(default: 0°)
W End angle—position of the last figure; reference: Z axis;
(default: 360°)
Wi Angle between figures
V
Direction—orientation (default: 0)
Z
C
H
 V=0, without W: Figures are arranged on a full circle
 V=0, with W: Figures are arranged on the longer circular arc
 V=0, with Wi: The algebraic sign of Wi defines the direction
(Wi<0: clockwise)
 V=1, with W: Clockwise
 V=1, with Wi: Clockwise (algebraic sign of Wi has no effect)
 V=2, with W: Counterclockwise
 V=2, with Wi: Counterclockwise (algebraic sign of Wi has no
effect)
Center of pattern
Center of pattern (angle)
Position of the figures (default: 0)
 H=0: Normal position—the figures are rotated about the circle
center (rotation)
 H=1: Original position—the position of the figures relative to
the coordinate system remains unchanged (translation)
 Program the hole/figure in the following block without a
center. Exception: circular slot: See "Circular pattern
with circular slots" on page 227..
 The milling cycle (MACHINING section) calls the hole/
figure in the following block—not the pattern definition.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
247
4.9 Tool positioning
4.9 Tool positioning
Rapid traverse G0
G0 moves at rapid traverse along the shortest path to the target point.
Parameters
X
Target point (diameter)
Z
Target point
Programming X, Z: Absolute, incremental or modal
If more axes are available on your machine, additional
input parameters will be displayed, e.g. parameter B for
the B axis.
Rapid traverse to machine coordinates G701
G701 moves at rapid traverse along the shortest path to the target
point.
Parameters
X
End point (diameter)
Z
End point
X, Z refer to the machine zero point and the slide zero
point.
If more axes are available on your machine, additional
input parameters will be displayed, e.g. parameter B for
the B axis.
248
DIN Programming
4.9 Tool positioning
Approach tool change point G14
G14 moves the slide at rapid traverse to the tool change position. In
setup mode, define permanent coordinates for the tool change
position.
Parameters
Q Sequence. Determines the course of traverse movements
(default: 0)
D
 0: Diagonal path of traverse
 1: First X, then Z direction
 2: First Z, then X direction
 3: Only X direction, Z remains unchanged
 4: Only Z direction, X remains unchanged
Number of the tool change position to be approached (0-2)
(default =0, tool change position from parameters)
Beispiel: G14
...
N1 G14 Q0 [Move to tool change point]
N2 T3 G95 F0.25 G96 S200 M3
N3 G0 X0 Z2
...
Definition of tool-change point G140
G140 defines the position of the tool change point defined in D. This
position can be approached with G14.
Parameters
D Number of the tool change point (1-2)
X
Diameter—Position of the tool change point
Z
Length—Position of the tool change point
If X or Z parameters are missing, the values from the tool
change point parameter are entered.
Beispiel: G140
...
N1 G14 Q0 [Tool change position from
parameter]
N2 T3 G95 F0.25 G96 S200 M3
N3 G0 X40 Z10
N5 G140 D1 X100 Z100 [Set tool change pos. 1]
N6 G14 Q0 D1
[Move to tool change pos. 1]
N7 G140 D2 X150 [Set tool change pos. 2, use
Z from parameters]
N8 G14 Q0 D2 [Move to tool change pos. 2]
...
HEIDENHAIN MANUALplus 620, CNC PILOT 640
249
4.10 Linear and circular movements
4.10 Linear and circular movements
Linear movement G1
G1 moves the tool on a linear path at the feed rate to the "end point."
Parameters
X
End point (diameter)
Z
End point
AN Angle (angular direction: see help graphic)
Q
Point of intersection. End point if the line segment intersects a
circular arc (default: 0):
BR
BE
 0: Near point of intersection
 1: Far point of intersection
Chamfer/rounding. Defines the transition to the next contour
element. When entering a chamfer/rounding, program the
theoretical end point.
 No input: Tangential transition
 BR=0: No tangential transition
 BR>0: Radius of rounding
 BR<0: Width of chamfer
Special feed factor for chamfer/rounding arc (default: 1)
Special feed rate = active feed rate * BE (0 < BE <= 1)
Programming X, Z: Absolute, incremental, modal or "?"
If more axes are available on your machine, additional
input parameters will be displayed, e.g. parameter B for
the B axis.
250
DIN Programming
4.10 Linear and circular movements
Circular path G2/G3
G2/G3 moves the tool in a circular arc at the feed rate to the "end
point." The center dimensioning is incremental. Direction of rotation
(see help graphic):
 G2: In clockwise direction
 G3: In counterclockwise direction
Parameters
X
End point (diameter)
Z
End point
R
Radius (0 < R <= 200 000 mm)
I
Incremental center point (distance from starting point to center
point; radius)
K
Incremental center point (distance from starting point to center
point)
Q
Point of intersection. End point if the circular arc intersects a
line segment or another circular arc (default: 0):
BR
BE
 0: Near point of intersection
 1: Far point of intersection
Chamfer/rounding. Defines the transition to the next contour
element. When entering a chamfer/rounding, program the
theoretical end point.
 No input: Tangential transition
 BR=0: No tangential transition
 BR>0: Radius of rounding
 BR<0: Width of chamfer
Special feed factor for chamfer/rounding arc (default: 1)
Special feed rate = active feed rate * BE (0 < BE <= 1)
Programming X, Z: Absolute, incremental, modal or "?"
Beispiel: G2, G3
N1 T3 G95 F0.25 G96 S200 M3
N2 G0 X0 Z2
N3 G42
N4 G1 Z0
N5 G1 X15 B-0.5 E0.05
N6 G1 Z-25 B0
N7 G2 X45 Z-32 R36 B2
N8 G1 A0
N9 G2 X80 Z-80 R20 B5
N10 G1 Z-95 B0
N11 G3 X80 Z-135 R40 B0
N12 G1 Z-140
N13 G1 X82 G40
...
HEIDENHAIN MANUALplus 620, CNC PILOT 640
251
4.10 Linear and circular movements
Circular path G12/G13
G12/G13 moves the tool in a circular arc at the feed rate to the "end
point." The center dimensioning is absolute. Direction of rotation (see
help graphic):
 G12: In clockwise direction
 G13: In counterclockwise direction
Parameters
X
End point (diameter)
Z
End point
R
Radius (0 < R <= 200 000 mm)
I
Absolute center point (radius)
K
Absolute center point
Q
Point of intersection. End point if the circular arc intersects a line
segment or another circular arc (default: 0):
BR
BE
 0: Near point of intersection
 1: Far point of intersection
Chamfer/rounding. Defines the transition to the next contour
element. When entering a chamfer/rounding, program the
theoretical end point.
 No input: Tangential transition
 BR=0: No tangential transition
 BR>0: Radius of rounding
 BR<0: Width of chamfer
Special feed factor for chamfer/rounding arc (default: 1)
Special feed rate = active feed rate * BE (0 < BE <= 1)
Programming X, Z: Absolute, incremental, modal or "?"
252
DIN Programming
4.11 Feed rate, shaft speed
4.11 Feed rate, shaft speed
Speed limitation G26
G26: Main spindle; Gx26: Spindle x (x: 1 to 3)
The speed limitation remains in effect until the end of the program or
until a new value is programmed for G26/Gx26.
Parameters
S
(Maximum) speed
Beispiel: G26
...
N1 G14 Q0
N1 G26 S2000 [maximum speed]
N2 T3 G95 F0.25 G96 S200 M3
If S > "absolute maximum speed" (machine parameter),
the parameter value will apply.
N3 G0 X0 Z2
...
Reduce rapid traverse G48
The reduction of the rapid traverse rate remains in effect until the end
of the program or until G48 is programmed again without input values.
Parameters
F
Max. feed rate in mm/min for linear axes or °/min for rotary axes
D Number of the axis
 1: X
 2: Y
 3: Z
 4: U
 5: V
 6: W
 7: A
 8: B
 9: C
HEIDENHAIN MANUALplus 620, CNC PILOT 640
253
4.11 Feed rate, shaft speed
Interrupted feed G64
G64 interrupts the programmed feed for a short period of time. G64 is
a modal function.
Parameters
E
Pause duration (0.01 s < E < 99.99 s)
F
Feed duration (0.01 s < E < 99.99 s)
 For switch-on, program G64 with E and F.
 For switch-off, program G64 without parameters.
Beispiel: G64
...
N1 T3 G95 F0.25 G96 S200 M3
N2 G64 E0.1 F1 [Interrupted feed on]
N3 G0 X0 Z2
N4 G42
N5 G1 Z0
N6 G1 X20 B-0.5
N7 G1 Z-12
N8 G1 Z-24 A20
N9 G1 X48 B6
N10 G1 Z-52 B8
N11 G1 X80 B4 E0.08
N12 G1 Z-60
N13 G1 X82 G40
N14 G64 [Interrupted feed off]
...
Feed per tooth Gx93
Gx93 (x: spindle 1 to 3) defines the drive-dependent feed rate with
respect to the number of teeth of the cutter.
Parameters
F
Feed per tooth in mm/tooth or inch/tooth
Beispiel: G193
...
N1 M5
N2 T1 G197 S1010 G193 F0.08 M104
The actual value display shows the feed rate in mm/rev.
N3 M14
N4 G152 C30
N5 G110 C0
N6 G0 X122 Z-50
N7 G...
N8 G...
N9 M15
...
254
DIN Programming
4.11 Feed rate, shaft speed
Constant feed rate G94 (feed per minute)
G94 defines the feed rate independent of drive.
Parameters
F
Feed per minute in mm/min or in./min
Beispiel: G94
...
N1 G14 Q0
N2 T3 G94 F2000 G97 S1000 M3
N3 G0 X100 Z2
N4 G1 Z-50
...
Feed per revolution Gx95
G95: Main spindle; Gx95: Spindle x (x: 1 to 3)
Gx95 defines a drive-dependent feed rate.
Parameters
F
Feed rate in mm/revolution or inch/revolution
Beispiel: G95, Gx95
...
N1 G14 Q0
N2 T3 G95 F0.25 G96 S200 M3
N3 G0 X0 Z2
N5 G1 Z0
N6 G1 X20 B-0.5
...
HEIDENHAIN MANUALplus 620, CNC PILOT 640
255
4.11 Feed rate, shaft speed
Constant surface speed Gx96
G96: Main spindle; Gx96: Spindle x (x: 1 to 3)
The spindle speed is dependent on the X position of the tool tip or on
the diameter of the drilling or milling tool.
Parameters
S
Cutting speed in m/min or ft/min
Beispiel: G96, G196
...
N1 T3 G195 F0.25 G196 S200 M3
N2 G0 X0 Z2
N3 G42
If you call a drilling tool while a constant cutting speed is
active, the Steuerung automatically calculates the spindle
speed from the programmed cutting speed and activates
it with Gx97. To prevent inadvertent rotation of the
spindle, program the spindle speed first and then T.
N4 G1 Z0
N5 G1 X20 B-0.5
N6 G1 Z-12
N7 G1 Z-24 A20
N8 G1 X48 B6
N9 G1 Z-52 B8
N10 G1 X80 B4 E0.08
N11 G1 Z-60
N12 G1 X82 G40
...
Speed Gx97
G97: Main spindle; Gx97: Spindle x (x: 1 to 3)
Constant spindle speed.
Parameters
S
Speed in revolutions per minute
Beispiel: G97, G197
...
N1 G14 Q0
N2 T3 G95 F0.25 G97 S1000 M3
G26/Gx26 limits the spindle speed.
N3 G0 X0 Z2
N5 G1 Z0
N6 G1 X20 B-0.5
...
256
DIN Programming
4.12 Tool-tip and cutter radius compensation
4.12 Tool-tip and cutter radius
compensation
Tool-tip radius compensation (TRC)
If TRC is not used, the theoretical tool tip is the reference point for the
paths of traverse. This might lead to inaccuracies when the tool moves
along non-paraxial paths of traverse. The TRC function corrects
programmed paths of traverse.
The TRC (Q=0) reduces the feed rate for circular arcs if the shifted
radius < the original radius. The TRC corrects the special feed rate
when a rounding arc is machined as transition to the next contour
element.
Reduced feed rate = feed rate * (shifted radius / original radius)
Milling cutter radius compensation (MCRC)
When the MCRC function is not active, the system defines the center
of the cutter as the reference point for the paths of traverse. With the
MCRC function, the Steuerung accounts for the outside diameter of
the tool when moving along the programmed paths of traverse. The
recessing, roughing and milling cycles already include TRC/MCRC
calls. The TRC/MCRC must be switched off when these cycles are
called.
 If the tool radii are > than the contour radii, the TRC/
MCRC might cause tool path loops. Recommendation:
Use the finishing cycle G890 or milling cycle G840.
 Never program the MCRC during a perpendicular
approach to the machining plane.
G40: Switch off TRC/MCRC
G40 is used to deactivate TRC/MCRC. Please note:
 The TRC/MCRC remains in effect until a block with G40 is reached.
 The block containing G40, or the block after G40 only permits a
linear path of traverse (G14 is not permissible).
Function of the TRC/MCRC
...
N.. G0 X10 Z10
N.. G41
Activate TRC to the left of the contour
N.. G0 Z20
Path of traverse: from X10/Z10 to X10+TRC/
Z20+TRC
N.. G1 X20
The path of traverse is "shifted" by the TRC
N.. G40 G0 X30 Z30
Path of traverse from X20+TRC/Z20+TRC to X30/
Z30
...
HEIDENHAIN MANUALplus 620, CNC PILOT 640
257
4.12 Tool-tip and cutter radius compensation
G41/G42: Switch on TRC/MCRC
G41: Switch on TRC/MCRC—compensation of the tool-tip/cutter
radius to the left of the contour in traverse direction.
G42: Switch on TRC/MCRC—compensation of the tool-tip/cutter
radius to the right of the contour in traverse direction.
Parameters
Q Plane (default: 0)
Beispiel: G40, G41, G42
...
N1 T3 G95 F0.25 G96 S200 M3
N2 G0 X0 Z2
N3 G42 [TRC on, to the right of the contour]
H
 0: TRC on the turning plane (XZ plane)
 1: MCRC on the front face (XC plane)
 2: MCRC on the lateral surface (ZC plane)
 3: MCRC on the front face (XY plane)
 4: MCRC on the lateral surface (YZ plane)
Output (only with MCRC)—(default: 0)
N9 G1 Z-52 B8
O
 0: Intersecting areas which are programmed in directly
successive contour elements are not machined.
 1: The complete contour is machined—even if certain areas
are intersecting.
Feed rate reduction (default: 0)
 0: Feed rate reduction is active
 1: No feed rate reduction
...
N4 G1 Z0
N5 G1 X20 B-0.5
N6 G1 Z-12
N7 G1 Z-24 A20
N8 G1 X48 B6
N10 G1 X80 B4 E0.08
N11 G1 Z-60
N12 G1 X82 G4 [TRC off]
Please note:
 Program G41/G42 in a separate NC block.
 Program a straight line segment (G0/G1) after the block containing
G41/G42.
 The TRC/MCRC is taken into account from the next path of traverse.
258
DIN Programming
4.13 Zero point shifts
4.13 Zero point shifts
You can program several zero point shifts in one NC program. The
relationships of the coordinates (for blank/finished part, auxiliary
contours) are retained by the zero offset description.
G920 temporarily deactivates zero point shifts—G980 reactivates
them.
Overview of zero point shifts
G51:
Page 260
 Relative shift
 Programmed shift
 Reference: Previously defined workpiece zero point
G53/G54/G55:
Page 261
 Relative shift
 Shift defined in setup mode (offset)
 Reference: Previously defined workpiece zero point
G56:
Page 261
 Additive shift
 Programmed shift
 Reference: Workpiece zero point defined at present
G59:
Page 262
 Absolute shift
 Programmed shift
 Reference: Machine zero point
HEIDENHAIN MANUALplus 620, CNC PILOT 640
259
4.13 Zero point shifts
Zero point shift G51
G51 shifts the workpiece zero point by the defined value in the
selected axis. The shift is referenced to the workpiece zero point
defined in setup mode.
Parameters
X
Shift (radius)
Y
Shift (machine-dependent)
Z
Shift
U Shift (machine-dependent)
V
Shift (machine-dependent)
W Shift (machine-dependent)
Even if you shift the zero point several times with G51, it is always
referenced to the workpiece zero point defined in setup mode.
The zero point shift is valid until program end, or until it is canceled by
other zero point shifts.
Beispiel: G51
...
N1 T3 G95 F0.25 G96 S200 M3
N2 G0 X62 Z5
N3 G810 NS7 NE12 P5 I0.5 K0.2
N4 G51 Z-28 [zero point shift]
N5 G0 X62 Z-15
N6 G810 NS7 NE12 P5 I0.5 K0.2
N7 G51 Z-56 [zero point shift]
...
260
DIN Programming
4.13 Zero point shifts
Zero point offsets—Shift G53/G54/G55
G53, G54 and G55 shift the workpiece zero point by the offset values
defined in setup mode.
The shift is referenced to the workpiece zero point defined in setup
mode, even if you shift the zero point several times with G53, G54 and
G55.
The shift remains in effect until the end of the program or until it is
canceled by other zero point shifts.
Before using zero point shifts with G53, G54 and G55, you need to
define the offset values in setup mode (see "Defining offsets" in the
User's Manual).
A shift in X is entered as a radius.
Additive zero point shift G56
G56 shifts the workpiece zero point by the defined value in the
selected axis. The shift is referenced to the currently active workpiece
zero point.
Parameters
X
Shift (radius value)—(default: 0)
Y
Shift (machine-dependent)
Z
Shift
U Shift (machine-dependent)
V
Shift (machine-dependent)
W Shift (machine-dependent)
If you shift the workpiece zero point more than once with G56, the
shift is always added to the currently active zero point.
Beispiel: G56
...
N1 T3 G95 F0.25 G96 S200 M3
N2 G0 X62 Z5
N3 G810 NS7 NE12 P5 I0.5 K0.2
N4 G56 Z-28 [zero point shift]
N5 G0 X62 Z5
N6 G810 NS7 NE12 P5 I0.5 K0.2
N7 G56 Z-28 [zero point shift]
...
HEIDENHAIN MANUALplus 620, CNC PILOT 640
261
4.13 Zero point shifts
Absolute zero point shift G59
G59 sets the workpiece zero point to the defined value in the selected
axis. The new workpiece zero point remains in effect to the end of the
program.
Parameters
X
Shift (radius)
Y
Shift (machine-dependent)
Z
Shift
U Shift (machine-dependent)
V
Shift (machine-dependent)
W Shift (machine-dependent)
G59 cancels all previous zero point shifts (with G51, G56
or G59).
Beispiel: G59
...
N1 G59 Z256 [zero point shift]
N2 G14 Q0
N3 T3 G95 F0.25 G96 S200 M3
N4 G0 X62 Z2
...
262
DIN Programming
4.14 Oversizes
4.14 Oversizes
Switch off oversize G50
G50 switches off oversizes defined with G52-Geo for the following
cycle. Program G50 before the cycle.
To ensure compatibility, the G52 code is also supported for switching
off the oversizes. HEIDENHAIN recommends using G50 for new NC
programs.
Axis-parallel oversize G57
G57 defines different oversizes for X and Z. Program G57 before the
cycle call.
Parameters
X
Oversize X (diameter value)—only positive values
Z
Oversize Z—only positive values
G57 is effective in the following cycles. After cycle run, the oversizes
are
 deleted: G810, G820, G830, G835, G860, G869, G890
 not deleted: G81, G82, G83
If the oversizes are programmed with G57 and in the
cycle itself, the cycle oversizes apply.
Beispiel: G57
...
N1 T3 G95 F0.25 G96 S200 M3
N2 G0 X120 Z2
N3 G57 X0.2 Z0.5 [paraxial oversize]
N4 G810 NS7 NE12 P5
...
HEIDENHAIN MANUALplus 620, CNC PILOT 640
263
4.14 Oversizes
Contour-parallel oversize (equidistant) G58
G58 defines an equidistant oversize. Program G58 before the cycle
call. A negative oversize during finishing is permitted with G890.
Parameters
P
Oversize
G58 is effective in the following cycles. After cycle run, the oversizes
are
 deleted: G810, G820, G830, G835, G860, G869, G890
 not deleted: G83
If an oversize is programmed with G58 and in the cycle,
the oversize from the cycle is used.
Beispiel: G58
...
N1 T3 G95 F0.25 G96 S200 M3
N2 G0 X120 Z2
N3 G58 P2 [contour-parallel oversize]
N4 G810 NS7 NE12 P5
...
264
DIN Programming
4.15 Safety clearances
4.15 Safety clearances
Safety clearance G47
G47 defines the safety clearance for
 the turning cycles: G810, G820, G830, G835, G860, G869, G890.
 the drilling cycles G71, G72, G74.
 the milling cycles G840...G846.
Parameters
P
Safety clearance
G47 without parameters activates the parameter values defined in the
"Safety clearance G47" user parameter.
G47 replaces the safety clearance set in the machining
parameters or that set in G147.
Safety clearance G147
G147 defines the safety clearance for
 the milling cycles G840...G846.
 the drilling cycles G71, G72, G74.
Parameters
I
Safety clearance to the milling plane (only for milling operations)
K
Safety clearance in approach direction (feed)
G147 without parameters activates the parameter values defined in
the "Safety clearance G147.." user parameter.
G147 replaces the safety clearance set in the machining
parameters or that set in G47.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
265
4.16 Tools, compensations
4.16 Tools, compensations
Tool call T
The Steuerung displays the tool assignment defined in the TURRET
section. You can enter the T number directly or select it from the tool
list (switch with the Tool list soft key).
266
DIN Programming
4.16 Tools, compensations
Correction of cut (switching the tool edge
compensation) G148
G148 defines the values compensating for wear. DX, DZ become
effective after program start and after a T command.
Parameters
O Selection (default: 0)
 O=0: DX, DZ active—DS inactive
 O=1: DS, DZ active—DX inactive
 O=2: DX, DS active—DZ inactive
The cycles G860, G869, G879, G870, G890 automatically
take the "correct" wear compensation into account.
Beispiel: G148
...
N1 T3 G95 F0.25 G96 S160 M3
N2 G0 X62 Z2
N3 G0 Z-29.8
N4 G1 X50.4
N5 G0 X62
N6 G150
N7 G1 Z-20.2
N8 G1 X50.4
N9 G0 X62
N10 G151
[recessing finishing]
N11 G148 O0 [change compensation]
N12 G0 X62 Z-30
N13 G1 X50
N14 G0 X62
N15 G150
N16 G148 O2
N17 G1 Z-20
N18 G1 X50
N19 G0 X62
...
HEIDENHAIN MANUALplus 620, CNC PILOT 640
267
4.16 Tools, compensations
Additive compensation G149
The Steuerung manages 16 tool-independent compensation values.
One G149 followed by a D number activates the additive
compensation function. G149 D900 deactivates the additive
compensation function. The compensation values are managed in the
Program Run mode (see "Program Run mode" in the User's Manual).
Parameters
D Additive compensation (default: D900):
 D900: deactivates the additive compensation
 D901 to D916: activates the additive compensation
Beispiel: G149
...
N1 T3 G96 S200 G95 F0.4 M4
N2 G0 X62 Z2
N3 G89
N4 G42
N5 G0 X27 Z0
Programming:
N6 G1 X30 Z-1.5
 The compensation becomes effective after the tool has moved in
the compensation direction by the compensation value. Therefore,
program G149 one block before the block containing the path of
traverse to which the compensation is to apply.
 Additive compensation remains in effect up to:
 the next G149 D900
 the next tool change
 End of program
N7 G1 Z-25
The additive compensation is added to the tool
compensation.
N8 G149 D901 [activate compensation]
N9 G1 X40 BR-1
N10 G1 Z-50
N11 G149 D902
N12 G1 X50 BR-1
N13 G1 Z-75
N14 G149 D900 [deactivate compensation]
N15 G1 X60 B-1
N16 G1 Z-80
N17 G1 X62
N18 G80
...
268
DIN Programming
4.16 Tools, compensations
Compensation of right-hand tool tip G150
Compensation of left-hand tool tip G151
G150/G151 defines the tool reference point for recessing and button
tools.
 G150: Reference point on right tip
 G151: Reference point on left tip
G150/G151 is effective from the block in which it is programmed and
remains in effect up to
 the next tool change
 program end.
 The displayed actual values always refer to the tool tip
defined in the tool data.
 If you use TRC, after G150/G151 you must also adjust
G41/G42.
Beispiel: G150, G151
...
N1 T3 G95 F0.25 G96 S160 M3
N2 G0 X62 Z2
N3 G0 Z-29.8
N4 G1 X50.4
N5 G0 X62
N6 G150
N7 G1 Z-20.2
N8 G1 X50.4
N9 G0 X62
N10 G151 [recessing finishing]
N11 G148 O0
N12 G0 X62 Z-30
N13 G1 X50
N14 G0 X62
N15 G150
N16 G148 O2
N17 G1 Z-20
N18 G1 X50
N19 G0 X62
...
HEIDENHAIN MANUALplus 620, CNC PILOT 640
269
4.17 Contour-based turning cycles
4.17 Contour-based turning cycles
Working with contour-based cycles
Possibilities of transferring the contour to be machined to the cycle:
Beispiel: Contour-based cycles
 Transferring the contour reference in the start block number and the
end block number. The contour area is machined in the direction
"from NS to NE."
 Transferring the contour reference via the name of the auxiliary
contour (ID). The complete auxiliary contour is machined in the
direction of contour definition.
 Describing the contour with G80 in the block directly after the cycle
(see „Cycle end / Simple contour G80” on page 294).
 Describing the contour with G0, G1, G2 and G3 blocks directly after
the cycle. The contour is concluded by G80 without parameters.
...
Possibilities of defining the workpiece blank for calculating the number
of cutting passes:
N7 G810 P3 [predefined contour description]
 Defining a global workpiece blank in the BLANK program section.
Regeneration of the workpiece blank is automatically active. The
cycle uses the specified workpiece blank.
 If no workpiece blank is defined, the cycle calculates the blank from
the contour to be machined and the position of the tool during cycle
call. Contour follow-up is not active.
Finding the block references:

Place cursor in NS or NE input field

Press the soft key
Select the contour element:
 Use the horizontal arrow keys to select the contour
element

N1 G810 NS7 NE12 P3 [block reference]
N2 ...
N3 G810 ID"007" P3 [name of auxiliary
contour]
N4 ...
N5 G810 ID"007" NS9 NE7 P3 [combination]
N6 ...
N8 G80 XS60 ZS-2 XE90 ZE-50 AC10 WC10
BS3 BE-2 RC5 EC0
N9...
N10 G810 P3 [direct contour description]
N11 G0 X50 Z0
N12 G1 Z-62 BR4
N13 G1 X85 AN80 BR-2
N14 G1 Zi-5
N15 G80
N16 ...
...
Use the vertical arrow keys to switch between
contours (also face contours, etc.).
Switch between NS and NE:
Press the NS soft key

270

Press the NE soft key

Press the soft key to confirm the block number and
return to the dialog.
DIN Programming
4.17 Contour-based turning cycles
Cutting limits in X, Z
The tool position before the cycle call determines the effect of a
cutting limit. The Steuerung machines the area to the right or to the
left of the cutting limit, depending on which side the tool has been
positioned before the cycle is called.
A cutting limit restricts the contour area that can be
machined; it does not apply to the paths for approach and
departure.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
271
4.17 Contour-based turning cycles
Longitudinal roughing G810
G810 machines the defined contour area. The reference to the
contour to be machined can be transferred in the cycle parameters, or
the contour can be defined directly after the cycle call (see „Working
with contour-based cycles” on page 270). The contour to be machined
can contain various valleys. If required, the area to be machined is
divided into several sections.
Parameters
ID
Auxiliary contour—ID number of the contour to be machined
NS
Starting block number (beginning of contour section)
NE
End block number (end of contour section)
P
I
K
E
 NE not programmed: The contour element NS is machined
in the direction of contour definition.
 NS=NE programmed: The contour element NS is machined
opposite to the direction of contour definition.
Maximum infeed
Oversize in X direction (diameter value)—(default: 0)
Oversize in Z direction (default: 0)
Plunging behavior
H
 E=0: Descending contours are not machined
 E>0: Plunging feed rate
 No input: Feed rate reduction depending on the plunge
angle—maximum 50%
Cutting limit in X direction (diameter value)—(default: no
cutting limit)
Cutting limit in Z direction (default: no cutting limit)
Approach angle (reference: Z axis)—(default: 0°/180°; parallel
to Z axis)
Departure angle (reference: Z axis)—(default: 90°/270°;
perpendicular to Z axis)
Type of departure (default: 0)
Q
 0: With each cut (machine contour outline after each pass)
 1: With the last cut (retracts at 45°; contour smoothing after
last pass)
 2: No smoothing (retracts at 45°; no contour smoothing)
Type of retraction at cycle end (default: 0)
X
Z
A
W
 0: Returns to starting point (first X, then Z direction)
 1: Positions in front of the finished contour
 2: Retracts to safety clearance and stops
272
DIN Programming
4.17 Contour-based turning cycles
Parameters
V
Identifier beginning/end (default: 0). A chamfer/rounding arc
is machined:
D
U
 0: At beginning and end
 1: At beginning
 2: At end
 3: No machining
 4: Chamfer/rounding arc is machined—not the basic
element (prerequisite: contour section with one element)
Omit elements (see figure)
Cut line on horizontal element (default: 0):
O
 0: No (regular proportioning of cuts)
 1: Yes (may result in irregular proportioning of cuts)
Hide undercutting:
 0: Undercuts are machined
 1: Undercuts are not machined
B
Slide lead with 4-axis machining (not yet implemented)
XA, ZA Starting point of blank (only effective if no blank was
programmed):
 XA, ZA not programmed: The workpiece blank contour is
calculated from the tool position and the ICP contour.
 XA, ZA programmed: Definition of the corner point of the
workpiece blank.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
273
4.17 Contour-based turning cycles
The Steuerung uses the tool definition to distinguish between external
and internal machining.
 The tool radius compensation is active.
 A G57 oversize enlarges the contour (also inside
contours.
 A G58 oversize
 >0: Enlarges the contour
 <0: Is not offset
 G57/G58 oversizes are deleted after cycle end.
Cycle run
1 Calculates the areas to be machined and the cutting
segmentation.
2 Approaches workpiece for first pass from starting point, taking
the safety clearance into account (first in Z direction, then in X).
3 Moves at feed rate to target point Z.
4 Depending on H:
5
6
7
8
9
 H=0: Machines the contour outline
 H=1 or 2: Retracts at 45°
Returns at rapid traverse and approaches for next pass.
Repeats 3 to 5 until target point X has been reached.
If required, repeats 2 to 6 until all areas have been machined.
If H=1: Smoothes the contour
Retracts as programmed in Q.
274
DIN Programming
4.17 Contour-based turning cycles
Face roughing G820
G820 machines the defined contour area. The reference to the
contour to be machined can be transferred in the cycle parameters, or
the contour can be defined directly after the cycle call (see „Working
with contour-based cycles” on page 270). The contour to be machined
can contain various valleys. If required, the area to be machined is
divided into several sections.
Parameters
ID
Auxiliary contour—ID number of the contour to be machined
NS Starting block number (beginning of contour section)
NE End block number (end of contour section)
P
I
K
E
 NE not programmed: The contour element NS is machined
in the direction of contour definition.
 NS=NE programmed: The contour element NS is machined
opposite to the direction of contour definition.
Maximum infeed
Oversize in X direction (diameter value)—(default: 0)
Oversize in Z direction (default: 0)
Plunging behavior
H
 E=0: Descending contours are not machined
 E>0: Plunging feed rate
 No input: Feed rate reduction depending on the plunge
angle—maximum 50%
Cutting limit in X direction (diameter value)—(default: no
cutting limit)
Cutting limit in Z direction (default: no cutting limit)
Approach angle (reference: Z axis)—(default: 90°/270°;
perpendicular to Z axis)
Departure angle (reference: Z axis)—(default: 0°/180°; parallel
to Z axis)
Type of departure (default: 0)
Q
 0: With each cut (machine contour outline after each pass)
 1: With the last cut (retracts at 45°; contour smoothing after
last pass)
 2: No smoothing (retracts at 45°; no contour smoothing)
Type of retraction at cycle end (default: 0)
X
Z
A
W
 0: Returns to starting point, first Z, then X direction
 1: Positions in front of the finished contour
 2: Retracts to safety clearance and stops
HEIDENHAIN MANUALplus 620, CNC PILOT 640
275
4.17 Contour-based turning cycles
Parameters
V
Identifier beginning/end (default: 0). A chamfer/rounding arc
is machined:
D
U
 0: At beginning and end
 1: At beginning
 2: At end
 3: No machining
 4: Chamfer/rounding arc is machined—not the basic
element (prerequisite: contour section with one element)
Omit elements (see figure)
Cut line on vertical element (default: 0):
O
 0: No (regular proportioning of cuts)
 1: Yes (may result in irregular proportioning of cuts)
Hide undercutting:
 0: Undercuts are machined
 1: Undercuts are not machined
B
Slide lead with 4-axis machining (not yet implemented)
XA, ZA Starting point of blank (only effective if no blank was
programmed):
 XA, ZA not programmed: The workpiece blank contour is
calculated from the tool position and the ICP contour.
 XA, ZA programmed: Definition of the corner point of the
workpiece blank.
The Steuerung uses the tool definition to distinguish between external
and internal machining.
 The tool radius compensation is active.
 A G57 oversize enlarges the contour (also inside
contours.
 A G58 oversize
 >0: Enlarges the contour
 <0: Is not offset
 G57/G58 oversizes are deleted after cycle end.
276
DIN Programming
4.17 Contour-based turning cycles
Cycle run
1 Calculates the areas to be machined and the cutting
segmentation.
2 Approaches workpiece for first pass from starting point, taking
the safety clearance into account (first in X direction, then in Z).
3 Moves at feed rate to target point X.
4 Depending on H:
5
6
7
8
9
 H=0: Machines the contour outline
 H=1 or 2: Retracts at 45°
Returns at rapid traverse and approaches for next pass.
Repeats 3 to 5 until target point Z has been reached.
If required, repeats 2 to 6 until all areas have been machined.
If H=1: Smoothes the contour
Retracts as programmed in Q.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
277
4.17 Contour-based turning cycles
Contour-parallel roughing G830
G830 machines the contour area defined in "ID", or by "NS, NE", parallel
to the contour (see „Working with contour-based cycles” on page
270). The contour to be machined can contain various valleys. If
required, the area to be machined is divided into several sections.
Parameters
ID
Auxiliary contour—ID number of the contour to be machined
NS
Starting block number (beginning of contour section)
NE
End block number (end of contour section)
P
I
K
X
Z
A
W
Q
 NE not programmed: The contour element NS is machined
in the direction of contour definition.
 NS=NE programmed: The contour element NS is machined
opposite to the direction of contour definition.
Maximum infeed
Oversize in X direction (diameter value)—(default: 0)
Oversize in Z direction (default: 0)
Cutting limit in X direction (diameter value)—(default: no
cutting limit)
Cutting limit in Z direction (default: no cutting limit)
Approach angle (reference: Z axis)—(default: 0°/180°, parallel
to Z axis, or with facing tools: parallel to X axis)
Departure angle (reference: Z axis)—(default: 90°/270°,
perpendicular to Z axis, or with facing tools: perpendicular to X
axis)
Type of retraction at cycle end (default: 0)
 0: Returns to starting point (first X, then Z direction)
 1: Positions in front of the finished contour
 2: Retracts to safety clearance and stops
278
DIN Programming
4.17 Contour-based turning cycles
Parameters
V
Identifier beginning/end (default: 0). A chamfer/rounding arc
is machined:
B
D
J
H
 0: At beginning and end
 1: At beginning
 2: At end
 3: No machining
 4: Chamfer/rounding arc is machined—not the basic
element (prerequisite: contour section with one element)
Contour calculation
 0: Automatic
 1: Tool to the left (G41)
 2: Tool to the right (G42)
Omit elements (see figure)
Workpiece blank oversize (radius value)—active only if no
blank has been defined.
Contour-parallel—Type of cutting paths:
 0: Constant machining depth
 1: Equidistant cut lines
HR
Specify primary machining direction
XA, ZA Starting point of blank (only effective if no blank was
programmed):
 XA, ZA not programmed: The workpiece blank contour is
calculated from the tool position and the ICP contour.
 XA, ZA programmed: Definition of the corner point of the
workpiece blank.
The Steuerung uses the tool definition to distinguish between external
and internal machining.
 The tool radius compensation is active.
 A G57 oversize enlarges the contour (also inside
contours.
 A G58 oversize
 >0: Enlarges the contour
 <0: Is not offset
 G57/G58 oversizes are deleted after cycle end.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
279
4.17 Contour-based turning cycles
Cycle run
1 Calculates the areas to be machined and the cutting
segmentation.
2 Approaches workpiece for first pass from starting point, taking
the safety clearance into account.
3 Executes the first cut (roughing).
4 Returns at rapid traverse and approaches for next pass.
5 Repeats 3 to 4 until the complete area has been machined.
6 If required, repeats 2 to 5 until all areas have been machined.
7 Retracts as programmed in Q.
280
DIN Programming
4.17 Contour-based turning cycles
Contour cycle, bidirectional (contour-parallel
with neutral tool) G835
G835 machines the contour area defined in "ID", or by "NS, NE", parallel
to the contour and bidirectionally (see „Working with contour-based
cycles” on page 270). The contour to be machined can contain various
valleys. If required, the area to be machined is divided into several
sections.
Parameters
ID
Auxiliary contour—ID number of the contour to be machined
NS Starting block number (beginning of contour section)
NE End block number (end of contour section)
P
I
K
X
Z
A
W
Q
V
 NE not programmed: The contour element NS is machined
in the direction of contour definition.
 NS=NE programmed: The contour element NS is machined
opposite to the direction of contour definition.
Maximum infeed
Oversize in X direction (diameter value)—(default: 0)
Oversize in Z direction (default: 0)
Cutting limit in X direction (diameter value)—(default: no
cutting limit)
Cutting limit in Z direction (default: no cutting limit)
Approach angle (reference: Z axis)—(default: 0°/180°, parallel
to Z axis, or with facing tools: parallel to X axis)
Departure angle (reference: Z axis)—(default: 90°/270°,
perpendicular to Z axis, or with facing tools: perpendicular to X
axis)
Type of retraction at cycle end (default: 0)
 0: Returns to starting point (first X, then Z direction)
 1: Positions in front of the finished contour
 2: Retracts to safety clearance and stops
Identifier beginning/end (default: 0). A chamfer/rounding arc is
machined:
 0: At beginning and end
 1: At beginning
 2: At end
 3: No machining
 4: Chamfer/rounding arc is machined—not the basic
element (prerequisite: contour section with one element)
HEIDENHAIN MANUALplus 620, CNC PILOT 640
281
4.17 Contour-based turning cycles
Parameters
B
Contour calculation
D
J
H
 0: Automatic
 1: Tool to the left (G41)
 2: Tool to the right (G42)
Omit elements (see figure)
Workpiece blank oversize (radius value)—active only if no
blank has been defined.
Contour-parallel—Type of cutting paths:
 0: Constant machining depth
 1: Equidistant cut lines
XA, ZA Starting point of blank (only effective if no blank was
programmed):
 XA, ZA not programmed: The workpiece blank contour is
calculated from the tool position and the ICP contour.
 XA, ZA programmed: Definition of the corner point of the
workpiece blank.
The Steuerung uses the tool definition to distinguish between external
and internal machining.
 The tool radius compensation is active.
 A G57 oversize enlarges the contour (also inside
contours.
 A G58 oversize
 >0: Enlarges the contour
 <0: Is not offset
 G57/G58 oversizes are deleted after cycle end.
Cycle run
1 Calculates the areas to be machined and the cutting
segmentation.
2 Approaches workpiece for first pass from starting point, taking
the safety clearance into account.
3 Executes the first cut (roughing).
4 Approaches for the next pass and executes the next cut
(roughing) in the opposite direction.
5 Repeats 3 to 4 until the complete area has been machined.
6 If required, repeats 2 to 5 until all areas have been machined.
7 Retracts as programmed in Q.
282
DIN Programming
4.17 Contour-based turning cycles
Recessing G860
G860 machines the defined contour area. The reference to the
contour to be machined can be transferred in the cycle parameters, or
the contour can be defined directly after the cycle call (see „Working
with contour-based cycles” on page 270). The contour to be machined
can contain various valleys. If required, the area to be machined is
divided into several sections.
Parameters
ID
Auxiliary contour—ID number of the contour to be machined
NS Start block number
NE
 Beginning of the contour section, or
 Reference to a G22/G23-Geo recess
End block number (end of contour section)
I
K
Q
 NE not programmed: The contour element NS is machined
in the direction of contour definition.
 NS=NE programmed: The contour element NS is machined
opposite to the direction of contour definition.
 NE is inapplicable if the contour is defined by G22/G23-Geo
Oversize in X direction (diameter value)—(default: 0)
Oversize in Z direction (default: 0)
Action (default: 0)
X
Z
V
E
EC
D
 0: Roughing and finishing
 1: Only roughing
 2: Only finishing
Cutting limit in X direction (diameter value)—(default: no
cutting limit)
Cutting limit in Z direction (default: no cutting limit)
Identifier beginning/end (default: 0). A chamfer/rounding arc is
machined:
 0: At beginning and end
 1: At beginning
 2: At end
 3: No machining
Finishing feed rate (default: active feed rate)
Dwell time
Revolutions on recessing floor
HEIDENHAIN MANUALplus 620, CNC PILOT 640
283
4.17 Contour-based turning cycles
Parameters
H
Type of retraction at cycle end (default: 0)
 0: Return to starting point
 Axial recess: First Z, then X direction
 Radial recess: First X, then Z direction
B
P
O
 1: Positions in front of the finished contour
 2: Retracts to safety clearance and stops
Recessing width
Cutting depth by which one cut is fed.
Roughing, lift-off
U
 0: Lift-up at rapid
 1: Below 45°
Finishing of floor element
 0: Value from global parameter
 1: Dividing
 2: Complete
The Steuerung uses the tool definition to distinguish between external
and internal machining, or between radial and axial recesses.
Contour cycle repeats can be programmed with G741 before the cycle
call.
 The tool radius compensation is active.
 A G57 oversize enlarges the contour (also inside
contours.
 A G58 oversize
 >0: Enlarges the contour
 <0: Is not offset
 G57/G58 oversizes are deleted after cycle end.
Cycle run (where Q=0 or 1)
1 Calculates the areas to be machined and the cutting
segmentation.
2 Approaches workpiece for first pass from starting point, taking
the safety clearance into account.
3
4
5
6
7
 Radial recess: First Z, then X direction
 Axial recess: First X, then Z direction
Executes first cut (roughing).
Returns at rapid traverse and approaches for next pass.
Repeats 3 to 4 until the complete area has been machined.
If required, repeats 2 to 5 until all areas have been machined.
If Q=0: Finish-machines the contour.
284
DIN Programming
4.17 Contour-based turning cycles
Repeat recessing cycle G740/G741
G740 and G741 are programmed before G860 to repeat the recessing
contour defined in Cycle G860.
Parameters
X
Starting point X (diameter value). Shifts the starting point of the
recessing contour defined by G860 to this coordinate.
Z
Starting point Z. Shifts the starting point of the recessing
contour defined by G860 to this coordinate.
I
Distance between the first and last recessing contour (X
direction).
K
Distance between the first and last recessing contour (Z
direction).
Ii
Distance between the recessing contours (X direction).
Ki
Distance between the recessing contours (Z direction).
Q
Number of recessing contours
A
Angle at which the recessing contours are arranged.
R
Length. Distance between the first and last recessing contour.
Ri
Length. Distance between the recessing contours.
Beispiel: G740, G741
...
The following parameter combinations are allowed:
AUXILIARY CONTOUR ID"recess"
 I, K
 Ii, Ki
 I, A
 K, A
 A, R
N 47 G0 X50 Z0
G740 does not support the parameters A and R.
MACHINING
N 48 G1 Z-5
N 49 G1 X45
N 54 G1 Z-15
N 56 G1 Z-17
N 162 T4
N 163 G96 S150 G95 F0.2 M3
N 165 G0 X120 Z100
N 166 G47 P2
N 167 G741 K-50 Q3 A180
N 168 G860 I0.5 K0.2 E0.15 Q0 H0
N 172 G0 X50 Z0
N 173 G1 X40
N 174 G1 Z-9
N 175 G1 X50
N 169 G80
N 170 G14 Q0
...
HEIDENHAIN MANUALplus 620, CNC PILOT 640
285
4.17 Contour-based turning cycles
Recess turning cycle G869
G869 machines the defined contour area. The reference to the
contour to be machined can be transferred in the cycle parameters, or
the contour can be defined directly after the cycle call (see „Working
with contour-based cycles” on page 270).
The workpiece is machined by alternate recessing and roughing
movements. The machining process requires a minimum of retraction
and infeed movements. The contour to be machined can contain
various valleys. If required, the area to be machined is divided into
several sections.
Parameters
ID
Auxiliary contour—ID number of the contour to be machined
NS
Start block number
NE
 Beginning of the contour section, or
 Reference to a G22/G23-Geo recess
End block number (end of contour section)
P
R
I
K
X
Z
A
W
Q
 NE not programmed: The contour element NS is machined
in the direction of contour definition.
 NS=NE programmed: The contour element NS is machined
opposite to the direction of contour definition.
 NE is inapplicable if the contour is defined by G22/G23-Geo
Maximum infeed
Turning depth compensation for finishing (default: 0)
Oversize in X direction (diameter value)—(default: 0)
Oversize in Z direction (default: 0)
Cutting limit (diameter value)—(default: no cutting limit)
Cutting limit (default: no cutting limit)
Approach angle (default: opposite to recessing direction)
Departure angle (default: opposite to recessing direction)
Action (default: 0)
U
 0: Roughing and finishing
 1: Only roughing
 2: Only finishing
Unidirectional turning (default: 0)
 0: The roughing passes are bidirectional.
 1: The roughing passes are unidirectional (from NS to NE)
286
DIN Programming
4.17 Contour-based turning cycles
Parameters
H
Type of retraction at cycle end (default: 0)
V
O
E
B
XA,
ZA
 0: Return to starting point (axial recess: first Z, then X
direction; radial recess: first X, then Z direction)
 1: Positions in front of the finished contour
 2: Retracts to safety clearance and stops
Identifier beginning/end (default: 0). A chamfer/rounding arc is
machined:
 0: At beginning and end
 1: At beginning
 2: At end
 3: No machining
Recessing feed rate (default: active feed rate)
Finishing feed rate (default: active feed rate)
Offset width (default: 0)
Starting point of blank (only effective if no blank was
programmed):
 XA, ZA not programmed: The workpiece blank contour is
calculated from the tool position and the ICP contour.
 XA, ZA programmed: Definition of the corner point of the
workpiece blank.
The Steuerung uses the tool definition to distinguish between radial
and axial recesses.
Program at least one contour reference (e.g.: NS or NS, NE) and P.
Turning depth compensation R: Depending on factors such as
workpiece material or feed rate, the tool tip is displaced during a
turning operation. You can correct the resulting infeed error with the
turning depth compensation factor. The value is usually determined
empirically.
Offset width B: After the second infeed movement, during the
transition from turning to recessing, the path to be machined is
reduced by "offset width B." Each time the system switches on this
side, the path is reduced by B—in addition to the previous offset. The
total offset is limited to 80 % of the effective cutting width (effective
cutting width = cutting width –2*cutting radius). If required, the
Steuerung reduces the programmed offset width. After clearance
roughing, the remaining material is removed with a single cut.
 The tool radius compensation is active.
 A G57 oversize enlarges the contour (also inside
contours.
 A G58 oversize
 >0: Enlarges the contour
 <0: Is not offset
 G57/G58 oversizes are deleted after cycle end.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
287
4.17 Contour-based turning cycles
Cycle run (where Q=0 or 1)
1 Calculates the areas to be machined and the cutting
segmentation.
2 Approaches workpiece for first pass from starting point, taking the
safety clearance into account.
3
4
5
6
7
 Radial recess: First Z, then X direction
 Axial recess: First X, then Z direction
Executes the first cut (recessing).
Machines perpendicularly to recessing direction (turning).
Repeats 3 to 4 until the complete area has been machined.
If required, repeats 2 to 5 until all areas have been machined.
If Q=0: Finish-machines the contour.
Machining information:
 Transition from turning to recessing: Before the transition from
turning to recessing, the Steuerung retracts the tool by 0.1 mm.
Thus an offset cutting edge is adjusted for the recessing operation,
independent of "offset width B."
 Inside radii and chamfers: Depending on the recessing width and
the radii of rounding arcs, single cuts preventing a "fluid transition"
from recessing to turning are executed before the rounding is
machined. This prevents damage to the tool.
 Edges: Edges are recessed. This prevents residual rings.
288
DIN Programming
4.17 Contour-based turning cycles
Recessing cycle G870
G870 generates a recess defined by G22-Geo. The Steuerung uses
the tool definition to distinguish between external and internal
machining, or between radial and axial recesses.
Parameters
ID
Auxiliary contour—ID number of the contour to be machined
NS Block number (reference to G22-Geo)
I
Oversize for roughing (default: 0)
E
 I=0: Recess is made in one work step.
 I>0: The first operation is roughing, the second finishing.
Dwell time (default: time for one spindle revolution)
 If I=0: For every recess
 If I>0: Only for finishing
Calculation of cutting segmentation:
Maximum offset = 0.8 * cutting width
 The tool radius compensation is active.
 An oversize is not taken into account.
Cycle run
1 Calculates the number of cutting passes.
2 Approaches workpiece from starting point for first pass.
3
4
5
6
7
 Radial recess: First Z, then X direction
 Axial recess: First X, then Z direction
Executes the first cut according to I.
Returns at rapid traverse and approaches for next pass.
If I=0: Dwells for time E
Repeats 3 to 4 until the complete recess has been machined.
If I>0: Finish machines the contour
HEIDENHAIN MANUALplus 620, CNC PILOT 640
289
4.17 Contour-based turning cycles
Finish contour G890
G890 finishes the defined contour area in one pass. The reference to
the contour to be machined can be transferred in the cycle
parameters, or the contour can be defined directly after the cycle call
(see „Working with contour-based cycles” on page 270). The contour
to be machined can contain various valleys. If required, the area to be
machined is divided into several sections.
Parameters
ID
Auxiliary contour—ID number of the contour to be machined
NS
Starting block number (beginning of contour section)
NE
End block number (end of contour section)
E
V
Q
 NE not programmed: The contour element NS is machined
in the direction of contour definition.
 NS=NE programmed: The contour element NS is machined
opposite to the direction of contour definition.
Plunging behavior
 E=0: Descending contours are not machined
 E>0: Plunging feed rate
 No input: Descending contours are machined at
programmed feed rate
Identifier beginning/end (default: 0). A chamfer/rounding arc is
machined:
 0: At beginning and end
 1: At beginning
 2: At end
 3: No machining
 4: Chamfer/rounding arc is machined—not the basic
element (prerequisite: contour section with one element)
Type of approach (default: 0)
 0: Automatic selection—the Steuerung checks:
 Diagonal approach
 First X, then Z direction
 Equidistant around the barrier
 Omission of the first contour elements if the starting
position is inaccessible
 1: First X, then Z direction
 2: First Z, then X direction
 3: No approach—tool is located near the starting point of the
contour area.
290
DIN Programming
4.17 Contour-based turning cycles
Parameters
H
Type of retraction (default: 3). Tool backs off at 45° against the
machining direction and moves as follows to the position I, K:
X
Z
D
I
K
O
U
B
 0: Diagonal
 1: First X, then Z direction
 2: First Z, then X direction
 3: Stops at safety clearance
 4: No retraction motion—tool remains on the end coordinate
 5: Diagonally to the tool position before the cycle call
 6: First in X, then in Z to the tool position before the cycle call
 7: First in Z, then in X to the tool position before the cycle call
Cutting limit (diameter value)—(default: no cutting limit)
Cutting limit (default: no cutting limit)
Omit elements (default: 1). Use the omit codes listed in the
table at right to omit individual elements, or the omit codes
listed in the table at the lower right to skip execution of
recesses, undercuts and relief turns.
End point that is approached at the end of the cycle (diameter
value)
End point that is approached at the end of the cycle
Feed rate reduction for circular elements (default: 0)
 0: Feed rate reduction is active
 1: No feed rate reduction
Cycle type—Required for generating the contour from the G80
parameters. (Default: 0)
 0: Standard contour (longitudinal or transverse), recessing
contour or ICP contour
 1: Linear path without/with return
 2: Circular arc CW, without/with return
 3: Circular arc CCW, without/with return
 4: Chamfer without/with return
 5: Rounding arc without/with return
Tool-tip radius compensation (default: 0)
 0: Automatic determination
 1: To the left of the contour
 2: To the right of the contour
 3: Automatic determination without taking the tool angle into
account
 4: To the left of the contour without taking the tool angle into
account
 5: To the right of the contour without taking the tool angle
into account
Codes for omitting recesses and undercuts
G call
Function
D code
G22
Recess for sealing ring
512
G22
Recess for guard ring
1.024
G23 H0
General recess
256
G23 H1
Relief turn
2.048
G25 H4
Undercut type U
32.768
G25 H5
Undercut type E
65.536
G25 H6
Undercut type F
131.072
G25 H7
Undercut type G
262.744
G25 H8
Undercut type H
524.288
G25 H9
Undercut type K
1.048.576
Add the codes if you want to hide several elements.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
291
4.17 Contour-based turning cycles
Parameters
HR Main cutting direction (default: 0)
 0: Automatic
 1: +Z
 2: +X
 3: -Z
 4: -X
The Steuerung uses the tool definition to distinguish between external
and internal machining.
Undercuts are machined if they are programmed and if tool geometry
permits.
Feed rate reduction
 For chamfers/rounding arcs, the following applies:
 Feed rate is programmed with G95-Geo: No automatic feed rate
reduction.
 Feed rate is not programmed with G95-Geo: Automatic feed rate
reduction. Each chamfer/rounding is therefore machined with at
least three revolutions.
 For chamfers/rounding arcs which, as a result of their size, are
machined with at least three revolutions, the feed rate is not
reduced automatically.
 For circular elements, the following applies:
 For small circular elements, the feed rate is decreased until every
element is machined with at least four spindle revolutions. You
can switch this feed rate reduction off with O.
 The tool radius compensation (TRC) results under certain
conditions in a feed rate reduction for circular elements (See "Tooltip and cutter radius compensation" on page 257.). You can switch
this feed rate reduction off with O.
 A G57 oversize enlarges the contour (also inside
contours.
 A G58 oversize
 >0: Enlarges the contour
 <0: Reduces the contour
 G57/G58 oversizes are deleted after cycle end.
292
DIN Programming
4.17 Contour-based turning cycles
Measuring cut G809
Cycle G809 performs a cylindrical measuring cut with the length
defined in the cycle, moves to the breakpoint for measuring and stops
the program. After the program was stopped, you can manually
measure the workpiece.
Parameters
X
Starting point X
Z
Starting point Z
R
Measuring cut length
P
Measuring cut oversize
I
Breakpoint Xi for measuring: Incremental distance to starting
point of measurement
K
Breakpoint Zi for measuring: Incremental distance to starting
point of measurement
ZS
Workpiece blank starting point: Collision-free approach for
inside machining
XE
Departing position X
D
Number of an additive compensation to be active during the
measuring cut
V
Measuring cut counter: Number of workpieces after which a
measurement is performed
Q
Machining direction
EC
 0: -Z
 1: +Z
Machining location
WE
 0: Outside
 1: Inside
Directions
O
 0: Simultaneously
 1: First X, then Z
 2: First Z, then X
Approach angle: If an approach angle is entered, the cycle
positions the tool over the starting point taking into account the
safety clearance, and from there plunges at the specified angle
to the diameter to be measured.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
293
4.18 Contour definitions in the machining section
4.18 Contour definitions in the
machining section
Cycle end / Simple contour G80
By programming G80 (with parameters), a turning contour consisting
of more than one element can be defined in one NC block. G80
(without parameters) ends a contour definition directly after a cycle.
Parameters
XS
Starting point of contour in X (diameter value)
ZS
Starting point of contour in Z
XE
Contour end point in X (diameter value)
ZE
Contour end point in Z
AC Angle of 1st element (range: 0° <= AC < 90°)
WC Angle of 2nd element (range: 0° <= AC <90°)
BS
Chamfer/rounding arc at starting point
WS Angle for chamfer at starting point
BE
Chamfer/rounding arc at end point
WE Angle for chamfer at end point
RC Radius
IC
Chamfer width
KC
Chamfer width
JC
Execution (see cycle programming)
EC
 0: Simple contour
 1: Expanded contour
Plunging contour
HC
 0: Rising contour
 1: Plunging contour
Contour direction for finishing:
 0: Longitudinal
 1: Transverse
"IC" and "KC" are used in the control to show the chamfer/rounding
cycles.
Beispiel: G80
N1 T3 G95 F0.25 G96 S200 M3
N2 G0 X120 Z2
N3 G810 P3
N4 G80 XS60 ZS-2 XE90 ZE-50 BS3 BE-2 RC5
N5 ...
N6 G0 X85 Z2
N7 G810 P5
N8 G0 X0 Z0
N9 G1 X20
N10 G1 Z-40
N11 G80
294
DIN Programming
4.18 Contour definitions in the machining section
Linear slot on front/rear face G301
G301 defines a linear slot in a contour on the front or rear face.
Program this figure in conjunction with G840, G845 or G846.
Parameters
XK Center in Cartesian coordinates
YK Center in Cartesian coordinates
X
Diameter (center point in polar coordinates)
C
Angle (center point in polar coordinates)
A
Angle to XK axis (default: 0°)
K
Slot length
B
Slot width
P
Depth/Height
 P<0: Pocket
 P>0: Island
Circular slot on front/rear face G302/G303
G302/G303 defines a circular slot in a contour on the front face/rear
face. Program this figure in conjunction with G840, G845 or G846.
 G302: Circular slot clockwise
 G303: Circular slot counterclockwise
Parameters
I
Center of curvature in Cartesian coordinates
J
Center of curvature in Cartesian coordinates
X
Diameter (center point in polar coordinates)
C
Angle (center point in polar coordinates)
R
Curvature radius (reference: center point path of the slot)
A
Starting angle; reference: XK axis (default: 0°)
W End angle; reference: XK axis (default: 0°)
B
Slot width
P
Depth/Height
 P<0: Pocket
 P>0: Island
HEIDENHAIN MANUALplus 620, CNC PILOT 640
295
4.18 Contour definitions in the machining section
Full circle on front/rear face G304
G304 defines a full circle in a contour on the front face/rear face.
Program this figure in conjunction with G840, G845 or G846.
Parameters
XK Center in Cartesian coordinates
YK Center in Cartesian coordinates
X
Diameter (center point in polar coordinates)
C
Angle (center point in polar coordinates)
R
Radius
P
Depth/Height
 P<0: Pocket
 P>0: Island
Rectangle on front/rear face G305
G305 defines a rectangle in a contour on the front face/rear face.
Program this figure in conjunction with G840, G845 or G846.
Parameters
XK
Center in Cartesian coordinates
YK
Center in Cartesian coordinates
X
Diameter (center point in polar coordinates)
C
Angle (center point in polar coordinates)
A
Angle to XK axis (default: 0°)
K
Length
B
(Height) width
R
Chamfer/rounding (default: 0°)
P
 R>0: Radius of rounding
 R<0: Width of chamfer
Depth/Height
 P<0: Pocket
 P>0: Island
296
DIN Programming
4.18 Contour definitions in the machining section
Eccentric polygon on front/rear face G307
G307 defines a polygon in a contour on the front face/rear face.
Program this figure in conjunction with G840, G845 or G846.
Parameters
XK Center in Cartesian coordinates
YK Center in Cartesian coordinates
X
Diameter (center point in polar coordinates)
C
Angle (center point in polar coordinates)
A
Angle of a polygon edge to XK axis (default: 0°)
Q
Number of edges (Q > 2)
K
Edge length
R
 K>0: Edge length
 K<0: Inscribed circle diameter
Chamfer/rounding (default: 0°)
P
 R>0: Radius of rounding
 R<0: Width of chamfer
Depth/Height
 P<0: Pocket
 P>0: Island
Linear slot on lateral surface G311
G311 defines a linear slot in a lateral-surface contour. Program this
figure in conjunction with G840, G845 or G846.
Parameters
Z
Center (Z position)
CY Center as linear value; reference: unrolled reference diameter
C
Center (angle)
A
Angle to Z axis (default: 0°)
K
Slot length
B
Slot width
P
Depth of pocket
HEIDENHAIN MANUALplus 620, CNC PILOT 640
297
4.18 Contour definitions in the machining section
Circular slot on lateral surface G312/G313
G312/G313 defines a circular slot in a lateral-surface contour. Program
this figure in conjunction with G840, G845 or G846.
 G312: Circular slot clockwise
 G313: Circular slot counterclockwise
Parameters
Z
Center
CY Center as linear value; reference: unrolled reference diameter
C
Center (angle)
R
Radius; reference: center point path of the slot
A
Starting angle; reference: Z axis (default: 0°)
W
End angle; reference: Z axis
B
Slot width
P
Depth of pocket
Full circle on lateral surface G314
G314 defines a full circle in a lateral-surface contour. Program this
figure in conjunction with G840, G845 or G846.
Parameters
Z
Center
CY Center as linear value; reference: unrolled reference diameter
C
Center (angle)
R
Radius
P
Depth of pocket
298
DIN Programming
4.18 Contour definitions in the machining section
Rectangle, lateral surface G315
G315 defines a rectangle in a lateral-surface contour. Program this
figure in conjunction with G840, G845 or G846.
Parameters
Z
Center
CY Center as linear value; reference: unrolled reference diameter
C
Center (angle)
A
Angle to Z axis (default: 0°)
K
Length
B
Width
R
Chamfer/rounding (default: 0°)
P
 R>0: Radius of rounding
 R<0: Width of chamfer
Depth of pocket
Eccentric polygon, lateral surface G317
G317 defines a polygon in a lateral-surface contour. Program this
figure in conjunction with G840, G845 or G846.
Parameters
Z
Center
CY Center as linear value; reference: unrolled reference diameter
C
Center (angle)
Q
Number of edges (Q > 2)
A
Angle to Z axis (default: 0°)
K
Edge length
R
 K>0: Edge length
 K<0: Inscribed circle diameter
Chamfer/rounding (default: 0°)
P
 R>0: Radius of rounding
 R<0: Width of chamfer
Depth of pocket
HEIDENHAIN MANUALplus 620, CNC PILOT 640
299
4.19 Thread cycles
4.19 Thread cycles
Overview of threading cycles
 G31 machines single threads, successions of threads and multi-start
threads defined with G24-Geo, G34-Geo or G37-Geo (FINISHED
PART). G31 can also machine a threading contour defined directly
after the cycle call and concluded by G80: See "Thread cycle G31" on
page 303.
 G32 cuts a single thread in any desired direction and position: See
"Single thread cycle G32" on page 307.
 G33 conducts a single thread cut. The direction of the single thread
cut is as desired: See "Thread single path G33" on page 309.
 G35 cuts a simple cylindrical metric ISO thread without run-out: See
"Metric ISO thread G35" on page 311.
 cuts a tapered API thread: See "Tapered API thread G352" on
page 312.
Handwheel superimposition
If your machine features handwheel superimposition, you can overlap
axis movements during thread cutting in a limited area:
 X direction: Maximum programmed thread depth depending on the
current cutting depth
 Z direction: +/- a fourth of the thread pitch
Machine and control must be specially prepared by the
machine tool builder for use of this cycle. Refer to your
machine manual.
Remember that position changes resulting from
handwheel superimposition are no longer effective after
the cycle end or the "last cut" function.
300
DIN Programming
4.19 Thread cycles
Parameter V: Type of infeed
With the V parameter you define the type of infeed for thread cutting
cycles.
The following infeed types are available:
0: Constant mach. X-section
The control reduces the cutting depth after each infeed to
achieve a consistent chip cross section and removal rate.
1: Constant infeed
The control uses the same cutting depth for each infeed without
exceeding the maximum infeed I.
2: EPL with distribution of cuts
The control uses the thread pitch F1 and the constant shaft speed
S to calculate the cutting depth for a constant infeed. If the thread
depth is not a multiple of the cutting depth, the control uses the
depth of the remaining cut for the first infeed. With the
"distribution of remaining cuts," the control divides the last cutting
depth into four partial cuts. The first cut is half the calculated
cutting depth, the second is a quarter and the third and fourth
each are an eighth.
3: EPL without distribution of cuts
The control uses the thread pitch F1 and the constant shaft speed
S to calculate the cutting depth for a constant infeed. If the thread
depth is not a multiple of the cutting depth, the control uses the
depth of the remaining cut for the first infeed. All subsequent
infeeds are constant and correspond to the calculated cutting
depth.
4: MANUALplus 4110
The control performs the first infeed with the maximum infeed I.
To determine the subsequent cutting depths, the control uses
the formula gt = 2 * I * SQRT "current no. of cuts", where "gt" is
the absolute depth. The cutting depth decreases with each
infeed since the current number of cuts is incremented by 1 with
each infeed. If, as a result, the remaining cut depth R falls below
the value defined in R, the control uses the value from R as the
new constant cutting depth! If the thread depth is not a multiple
of the cutting depth, the control performs the last cut to the final
depth.
5: Constant infeed (4290)
The control uses the same cutting depth for each infeed; the
cutting depth corresponds to the maximum infeed I. If the thread
depth is not a multiple of the cutting depth, the control uses the
depth of the remaining cut for the first infeed.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
301
4.19 Thread cycles
6: Constant infeed with remaining cutting (4290)
The control uses the same cutting depth for each infeed; the
cutting depth corresponds to the maximum infeed I. If the thread
depth is not a multiple of the cutting depth, the control uses the
depth of the remaining cut for the first infeed. With the
"distribution of remaining cuts," the control divides the last cutting
depth into four partial cuts. The first cut is half the calculated
cutting depth, the second is a quarter and the third and fourth
each are an eighth.
302
DIN Programming
4.19 Thread cycles
Thread cycle G31
G31 machines single threads, successions of threads and multi-start
threads defined with G24-, G34- or G37-Geo. G31 can also machine a
threading contour defined directly after the cycle call and concluded by
G80.
Parameters
ID
Auxiliary contour—ID number of the contour to be machined
NS Contour start block number (reference to basic element G1Geo; for successions of threads: block number of the first
basic element)
NE Contour end block number (reference to basic element G1Geo; for successions of threads: block number of the last basic
element)
O
Identifier beginning/end (default: 0). A chamfer/rounding arc is
machined:
J
 0: No machining
 1: At beginning
 2: At end
 3: At beginning and end
 4: Chamfer/rounding arc is machined—not the basic
element (prerequisite: contour section with one element)
Reference direction:
I
 No input: The reference direction is determined from the
first contour element.
 J=0: Longitudinal thread
 J=1: Transverse thread
Maximum infeed
IC
No input and V=0 (constant chip cross section):
I = 1/3 * F
Number of cuts. The infeed is calculated from IC and U. Usable
with:
Beispiel: G31
...
B
 V=0 (constant chip cross section)
 V=1 (constant infeed)
Run-in length
N
2 G0 X16 Z0
N
3 G52 P2 H1
N
4 G95 F0.8
P
No input: The run-in length is determined from the contour. If
this is not possible, the value is calculated from the kinematic
parameters. The thread contour is extended by the value B.
Overrun length
N
5 G1 Z-18
N
6 G25 H7 I1.15 K5.2 R0.8 W30 BF0 BP0
N
7 G37 Q12 F2 P0.8 A30 W30
A
No input: The run-out length is determined from the contour. If
this is not possible, the value is calculated. The thread contour
is extended by the value P.
Approach angle (angle of infeed) (default: 30°)
N
8 G1 X20 BR-1 BF0 BP0
FINISHED
N 9 G1 Z-23.8759 BR0
N 10 G52 G95
N 11 G3 Z-41.6241 I-14.5 BR0
N 12 G1 Z-45
HEIDENHAIN MANUALplus 620, CNC PILOT 640
303
4.19 Thread cycles
Parameters
V
Type of infeed (default: 0); for details, see page 301
H
 0: Constant cross section for all cuts
 1: Constant infeed
 2: W/ remaining cutting (with distribution of remaining cuts).
First infeed = Remainder of the division of thread depth/
cutting depth. The last cut is divided into four partial cuts: 1/
2, 1/4, 1/8 and 1/8.
 3: Infeed is calculated from the pitch and spindle speed
 4: Same as MANUALplus 4110
 5: Constant infeed (same as 4290)
 6: Constant with distribute. (same as 4290)
Type of offset for smoothing the thread flanks (default: 0)
BD
 0: Without offset
 1: Offset from the left
 2: Offset from the right
 3: Tool is offset alternately from the right and left
Depth of remaining cuts—only in conjunction with approach
type V=4 (same as MANUALplus 4110)
Starting angle (thread start is defined with respect to
rotationally nonsymmetrical contour elements)—(default: 0)
External/internal thread (no meaning for closed contours)
F
U
K
 0: External thread
 1: Internal thread
Thread pitch
Thread depth
Run-out length
R
C
 K>0: Run-out
 K<0: Run-in
D
E
Q
The length K should be at least the value of the thread depth.
Number of thread turns for multi-start thread
Variable pitch (no effect at present)
Number of no-load (air) cuts after the last cut (for reducing the
cutting pressure in the thread base)—(default: 0)
If a thread has been defined with G24-Geo, G34-Geo or
G37-Geo, the parameters F, U, K and D are not relevant.
Beispiel: G31, continued
N 13 G1 X30 BR2
N 14 G1 Z-50 BR0
N 15 G2 X36 Z-71 I12 BR5
N 16 G1 X40 Z-80
N 17 G1 Z-99
N 18 G1 Z-100 [thread]
N 19 G1 X50
N 20 G1 Z-120
N 21 G1 X0 [thread]
N 22 G1 Z0
N 23 G1 X16 BR-1.5
...
AUXILIARY CONTOUR ID"thread"
N 24 G0 X20 Z0
N 25 G1 Z-30
N 26 G1 X30 Z-60
N 27 G1 Z-100
MACHINING
N 33
G14 Q0 M108
N 30
T9 G97 S1000 M3
N 34
G47 P2
N 35 G31 NS16 NE17 J0 IC5 B5 P0 V0 H1
BD0 F2 K10
N 36
G0 X110 Z20
N 38
G47 M109
[G80 contours can be inside or outside]
N 43 G31 IC4 B4 P4 A30 V0 H2 C30 BD0 F6
U3 K-10 Q2
N 44 G0 X80 Z0
N 45 G1 Z-20
N 46 G1 X100 Z-40
Run-in length B: The slide requires a run-in distance at the start of
thread in order to accelerate to the programmed contouring feed rate
before starting the actual thread.
Run-out length P: The slide needs an overtravel at the end of the
thread to decelerate again. Remember that the paraxial line P needs
overtravel even with an oblique thread run-out
304
N 47 G1 Z-60
N 48 G80
[External thread regardless of the value
defined in BD]
N 49
G0 X50 Z-30
DIN Programming
Run-in length: B = 0.75 * (F*S)² / a * 0.66 + 0.15
Run-out length: P = 0.75 * (F*S)² / a * 0.66 + 0.15
 F: Thread pitch in mm/revolution
 S: Speed in revolutions/second
 a: Acceleration in mm/s² (see axis data)
Beispiel: G31, continued
N 50 G31 NS16 NE17 O0 IC2 B4 P0 A30 V0
H1 C30 BD1 F2 U1 K10
N 51
N 52
Determination of external/internal thread:
 G31 with contour reference—closed contour: External or internal
thread is defined by the contour. BD has no meaning.
 G31 with contour reference—open contour: External or internal
thread is defined by "BD". If "BD" is not programmed, the contour is
used to determine whether a thread is external or internal.
 If the thread contour is programmed directly after the cycle, "BD"
determines whether the thread is an internal or external thread. If
"BD" is not programmed, the algebraic sign of "U" is evaluated (as in
the MANUALplus 4110).
 U>0: Internal thread
 U<0: External thread
G0 Z10 X50
[AUXILIARY CONTOURS can be inside or
outside if they are not closed contours]
G0 X50 Z-30
N 53 G31 ID"thread" O0 IC2 B4 P0 A30 V0
H1 C30 BD1 F2 U1 K10
N 60
G0 Z10 X50
Starting angle C: At the end of the "run-in path B" the spindle is at the
"starting angle C" position. Therefore, if the thread is to start exactly at
the starting angle, position the tool by the run-in length—or by the runin length plus a multiple of the thread pitch—in front of the beginning
of the thread.
The individual thread cuts are calculated from the thread depth,
maximum approach I and type of approach V.
 Cycle stop—the Steuerung retracts the tool from the
thread groove and then stops all tool movements. (Liftoff distance: OEM configuration parameter:
cfgGlobalProperties-threadliftoff)
 Feed rate override is not effective.
Danger of collision!
An excessive overrun length P might cause a collision. You
can check the overrun length during the simulation.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
305
4.19 Thread cycles
You can calculate the minimum run-in and run-out length with the
following equation.
4.19 Thread cycles
Cycle run
1
Calculates the number of cutting passes.
2
Moves diagonally to the internal starting point at rapid traverse.
This point lies in front of the "starting point of thread" by the runin length B. With H=1 (or 2, 3) the current offset is taken into
account for calculating the internal starting point.
3
4
5
6
7
8
9
306
The internal starting point is calculated on the basis of the tool
tip.
Accelerates to feed rate (line B).
Executes a thread cut.
Decelerates (line P).
Retracts to safety clearance, returns at rapid traverse, and
approaches for next pass. For multiple threads, the same rate of
cut is used for each thread turn, before the next infeed motion
is executed.
Repeats 3 to 6 until the complete thread has been cut.
Executes air cuts.
Returns to starting point.
DIN Programming
4.19 Thread cycles
Single thread cycle G32
G32 cuts a single thread in any desired direction and position
(longitudinal, tapered or transverse thread; internal or external thread).
Parameters
X
End point of thread (diameter)
Z
End point of thread
XS
Starting point for thread (diameter)
ZS
Starting point for thread
BD External/internal thread:
F
U
 0: External thread
 1: Internal thread
Thread pitch
Thread depth
No input: The thread depth is calculated automatically:
I
IC
 External thread (0.6134 * F)
 Internal thread (0.5413 * F)
Maximum cutting depth
Number of cuts. The infeed is calculated from IC and U. Usable
with:
V
 V=0 (constant chip cross section)
 V=1 (constant infeed)
Type of infeed (default: 0); for details, see page 301
H
 0: Constant cross section for all cuts
 1: Constant infeed
 2: W/ remaining cutting (with distribution of remaining cuts).
First infeed = Remainder of the division of thread depth/
cutting depth. The last cut is divided into four partial cuts: 1/
2, 1/4, 1/8 and 1/8
 3: Infeed is calculated from the pitch and spindle speed
 4: Same as MANUALplus 4110
 5: Constant infeed (same as 4290)
 6: Constant with distribute. (same as 4290)
Type of offset for smoothing the thread flanks (default: 0)
WE
 0: Without offset
 1: Offset from the left
 2: Offset from the right
 3: Tool is offset alternately from the right and left
Lift off method with K=0 (default: 0)
K
 0: G0 at end
 1: Lift-off in thread
Run-out length at thread end point (default: 0)
HEIDENHAIN MANUALplus 620, CNC PILOT 640
307
4.19 Thread cycles
Parameters
W
Taper angle (range: –45° < W < 45°)—(default: 0)
Position of the taper thread with respect to longitudinal or
transverse axis:
 W>0: Rising contour (in machining direction)
 W<0: Falling contour
Parameters
C
Starting angle (thread start is defined with respect to
rotationally nonsymmetrical contour elements)—(default: 0)
A
Approach angle (angle of infeed) (default: 30°)
R
Remainder cuts (default: 0)
E
Q
D
J
 0: The last cut is divided into four partial cuts: 1/2, 1/4, 1/8
and 1/8.
 1: W/o remaining cutting (without distribution of remaining
cuts)
Variable pitch (no effect at present)
Number of no-load (air) cuts after the last cut (for reducing the
cutting pressure in the thread base)—(default: 0)
Number of thread turns for multi-start thread
Reference direction:
 No input: The reference direction is determined from the
first contour element.
 J=0: Longitudinal thread
 J=1: Transverse thread
Beispiel: G32
...
N1 T4 G97 S800 M3
N2 G0 X16 Z4
N3 G32 X16 Z-29 F1.5 [thread]
The cycle calculates the thread from the thread end point, thread
depth and the tool position.
...
First infeed = Remainder of the division of thread depth/cutting depth.
Transverse threads: Use G31 with contour definition for cutting
transverse threads.
 Cycle stop—the Steuerung retracts the tool from the
thread groove and then stops all tool movements. (Liftoff distance: OEM configuration parameter:
cfgGlobalProperties-threadliftoff)
 Feed rate override is not effective.
Cycle run
1 Calculates the number of cutting passes.
2 Executes a thread cut.
3 Returns at rapid traverse and approaches for next pass.
4 Repeats 2 to 3 until the complete thread has been cut.
5 Executes air cuts.
6 Returns to starting point.
308
DIN Programming
4.19 Thread cycles
Thread single path G33
G33 conducts a single thread cut. The direction of the single thread
path is as desired (longitudinal, tapered or transverse threads; internal
or external threads). You can make successive threads by
programming G33 several times in succession.
Position the tool in front of the thread by the run-in length B if the slide
must accelerate to the feed rate. And remember the run-out length P
before the end point of thread if the slide has to be decelerated.
Parameters
X
End point of thread (diameter)
Z
End point of thread
F
Thread pitch
B
Slop. length (run-in length; length of the acceleration path)
P
Overflow length (run-out length; length of the deceleration
path)
C
Starting angle (thread start is defined with respect to
rotationally nonsymmetrical contour elements)—(default: 0)
H
Reference direction for thread pitch (default: 0)
E
I
K
 0: Feed rate on the Z axis (for longitudinal and taper threads
up to a max. angle of +45°/–45° to the Z axis)
 1: Feed rate on the X axis (for transverse and taper threads
up to a max. angle of +45°/–45° to the X axis)
 3: Contouring feed rate
Variable pitch (default: 0)—(no effect at present)
Retraction distance in X—retraction path for cycle stop in the
thread, incremental value
Retraction distance in Z—retraction path for cycle stop in the
thread, incremental value
Run-in length B: The slide requires a run-in distance at the start of
thread in order to accelerate to the programmed feed rate before
starting the actual thread.
Beispiel: G33
...
Default: cfgAxisProperties/SafetyDist
N1 T5 G97 S1100 G95 F0.5 M3
Run-out length P: The slide needs an overtravel at the end of the
thread to decelerate again. Remember that the paraxial line P needs
overtravel even with an oblique thread run-out
N2 G0 X101.84 Z5
 P=0: Start of a successive thread
 P>0: End of a successive thread
Starting angle C: At the end of the "run-in path B" the spindle is at the
"starting angle C" position.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
N3 G33 X120 Z-80 F1.5 P0 [thread single
path]
N4 G33 X140 Z-122.5 F1.5
N5 G0 X144
...
309
4.19 Thread cycles
 Cycle stop—the Steuerung retracts the tool from the
thread groove and then stops all tool movements. (Liftoff distance: OEM configuration parameter:
cfgGlobalPrperties-threadliftoff)
 Feed rate override is not effective
 Create thread with G95 (feed rate per revolution)
Cycle run
1 Accelerates to feed rate (line B).
2 Moves at feed rate to end point of thread –run-out length P.
3 Decelerates (line P) and stops at the end point of thread.
Activating handwheel during G33
With the G923 function you can activate the handwheel in order to
make compensations during a thread cut. In the G923 function you
define limits within which traverse with the handwheel is possible.
Parameters
X
Max. positive offset: Limit in +X
Z
Max. positive offset: Limit in +Z
U
Max. negative offset: Limit in –X
W
Max. negative offset: Limit in –Z
H
Reference direction:
Q
 H=0: Longitudinal thread
 H=1: Transverse thread
Thread type:
 Q=1: Right-hand thread
 Q=2: Left-hand thread
310
DIN Programming
4.19 Thread cycles
Metric ISO thread G35
G35 cuts a longitudinal thread (internal or external thread). The thread
starts at the current tool position and ends at the end point X, Z.
From the tool position relative to the end point of the thread, the
Steuerung automatically determines whether an internal or external
thread is to be cut.
Parameters
X
End point of thread (diameter)
Z
End point of thread
F
Thread pitch
I
Maximum infeed
Q
V
No input: I is calculated from the thread pitch and the thread
depth.
Number of no-load (air) cuts after the last cut (for reducing the
cutting pressure in the thread base)—(default: 0)
Type of infeed (default: 0); for details, see page 301
 0: Constant cross section for all cuts
 1: Constant infeed
 2: W/ remaining cutting (with distribution of remaining cuts).
First infeed = Remainder of the division of thread depth/
cutting depth. The last cut is divided into four partial cuts: 1/
2, 1/4, 1/8 and 1/8.
 3: Infeed is calculated from the pitch and spindle speed
 4: Same as MANUALplus 4110
 5: Constant infeed (same as 4290)
 6: Constant with distribute. (same as 4290)
 Cycle stop—the Steuerung retracts the tool from the
thread groove and then stops all tool movements. (Liftoff distance: OEM configuration parameter:
cfgGlobalPrperties-threadliftoff)
 If you are programming an internal thread, it is advisable
to preset the thread pitch F since the diameter of the
longitudinal element is not the thread diameter. If you
have the Steuerung calculate the thread pitch
automatically, slight deviations may occur.
Cycle run
1 Calculates the number of cutting passes.
2 Executes a thread cut.
3 Returns at rapid traverse and approaches for next pass.
4 Repeats 2 to 3 until the complete thread has been cut.
5 Executes air cuts.
6 Returns to starting point.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
Beispiel: G35
%35.nc
[G35]
N1 T5 G97 S1500 M3
N2 G0 X16 Z4
N3 G35 X16 Z-29 F1.5
END
311
4.19 Thread cycles
Tapered API thread G352
This cycle cuts a tapered single or multi-start API thread. The depth of
thread decreases at the overrun at the end of thread.
Parameters
X
End point of thread (diameter)
Z
End point of thread
XS
Starting point for thread (diameter)
ZS
Starting point for thread
F
Thread pitch
U
Thread depth
V
 U>0: Internal thread
 U<=0: External thread (lateral surface or front face)
 U= +999 or –999: Thread depth is calculated
Maximum approach (infeed) (default: I is calculated from the
thread pitch and the thread depth)
Type of infeed (default: 0); for details, see page 301
H
 0: Constant cross section for all cuts
 1: Constant infeed
 2: W/ remaining cutting (with distribution of remaining cuts).
First infeed = Remainder of the division of thread depth/
cutting depth. The last cut is divided into four partial cuts: 1/
2, 1/4, 1/8 and 1/8
 3: Infeed is calculated from the pitch and spindle speed
 4: Same as MANUALplus 4110
Type of offset for smoothing the thread flanks (default: 0)
A
 0: Without offset
 1: Offset from the left
 2: Offset from the right
 3: Tool is offset alternately from the right and left
Approach (infeed) angle (range: -60° < A < 60°; default: 30°)
I
R
W
WE
D
Q
C
312
 A>0: Infeed on right thread flank
 A<0: Infeed on left thread flank
Depth of remaining cuts—only in conjunction with approach
type V=4 (same as MANUALplus 4110)
Taper angle (range: –45° < W < 45°; default: 0°)
Run-out angle (range: 0° < WE < 90°; default: 12°)
Threads per unit (number of thread turns) for multi-start thread
Number of no-load (air) cuts after the last cut (for reducing the
cutting pressure in the thread base)—(default: 0)
Starting angle (thread start is defined with respect to
rotationally nonsymmetrical contour elements)—(default: 0)
Beispiel: G352
%352.nc
[G352]
N1 T5 G97 S1500 M3
N2 G0 X13 Z4
N3 G352 X16 Z-28 XS13 ZS0 F1.5 U-999
WE12
END
DIN Programming
4.19 Thread cycles
Internal or external threads: See algebraic sign of "U."
Number of cutting passes: The first cut is performed at the cutting
depth defined for "I" and is reduced with each cut until the tool reaches
the "remaining cutting depth R."
Handwheel superposition (provided that your machine is equipped
accordingly): The superposition is limited to the following range:
 X direction: Depending on the current cutting depth—without
exceeding the starting and end points of the thread.
 Z direction: Maximal 1 thread groove—without exceeding the
starting and end points of the thread.
Definition of taper angle:
 XS/ZS, X/Z
 XS/ZS, Z, W
 ZS, X/Z, W
 Cycle stop—the Steuerung retracts the tool from the
thread groove and then stops all tool movements. (Liftoff distance: OEM configuration parameter:
cfgGlobalPrperties-threadliftoff)
 If you are programming an internal thread, it is advisable
to preset the thread pitch F since the diameter of the
longitudinal element is not the thread diameter. If you
have the Steuerung calculate the thread pitch
automatically, slight deviations may occur.
Cycle run
1 Calculates the number of cutting passes.
2 Executes a thread cut.
3 Returns at rapid traverse and approaches for next pass.
4 Repeats 2 to 3 until the complete thread has been cut.
5 Executes air cuts.
6 Returns to starting point.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
313
4.19 Thread cycles
Metric ISO thread G38
Cycle G38 creates a cylindrical thread whose form does not
correspond to the tool form. Use a recessing or button tool for
machining.
Describe the contour of the thread turn as auxiliary contour. The
position of the auxiliary contour must correspond to the start position
of the thread cuts. You can select the entire auxiliary contour or just
segments in the cycle.
Parameters
ID
Name of the auxiliary contour
NS
Start block of the contour to be machined
NE
End block of the contour to be machined
Q
Thread depth
X
Z
F
I
 0: Roughing: The contour is roughed out line by line at
maximum infeed I and K. A programmed oversize (G58 or
G57) is taken into account.
 1: Finishing: The turn of the thread is created in individual
cuts along the contour. Define the distances between the
individual thread cuts on the contour with I and K.
End point of thread X
End point of thread Z
Thread pitch
Maximum infeed
K
 If Q=0: Plunging depth
 If Q=1: Distance between the finishing cuts as arc length
Maximum infeed
J
C
O
 If Q=0: Offset width
 If Q=1: Distance between the finishing cuts on straight line
Run-out length
Starting angle
Type of infeed
 0: Rapid traverse
 1: Feed rate
Beispiel: G38
%352.nc
[G38]
N1 T5 G97 S1500 M3
N2 G0 X43 Z4
N3 G38 ID"123" NS3 NE5 X40 Z-30 F1.5 I0.8
K0.5 J3 C0
END
314
DIN Programming
4.20 Parting cycle
4.20 Parting cycle
Cut-off cycle G859
Cycle G859 parts the workpiece. If programmed, a chamfer or
rounding arc is machined on the outside diameter. At the end of cycle,
the tool retracts and returns to the starting point.
You can define a feed rate reduction, which becomes effective as
soon as the position I is reached.
Parameters
X
Cut-off (parting) diameter
Z
Cut-off (parting) position
I
Diameter for feed rate reduction
XE
E
B
D
K
SD
U
 I is defined: The control switches to feed rate E after this
position
 I is not defined: No feed rate reduction
Inside diameter (pipe)
Reduced feed rate
Chamfer/rounding
 B>0: Radius of rounding
 B<0: Width of chamfer
Speed limitation: Maximum speed during parting
Retraction distance after parting: Lift off the tool laterally from
the plane surface before retraction
Speed limitation from the diameter I up
Diameter from which the part catcher is activated (machinedependent function)
Beispiel: G859
%859.nc
[G859]
N1 T3 G95 F0.23 G96 S248 M3
N2 G0 X60 Z-28
N3 G859 X50 Z-30 I10 XE8 E0.11 B1
END
HEIDENHAIN MANUALplus 620, CNC PILOT 640
315
4.21 Undercut cycles
4.21 Undercut cycles
Undercut cycle G85
With the function G85, you can machine undercuts according to
DIN 509 E, DIN 509 F and DIN 76 (thread undercut).
Parameters
X
Target point (diameter)
Z
Target point
I
Depth (radius)
K
E
 DIN 509 E, F: Grinding oversize (default: 0)
 DIN 76: Undercut depth
Undercut width and type of undercut
 K—No input: DIN 509 E
 K=0: DIN 509 F
 K>0: Undercut width for DIN 76
Reduced feed for machining the undercut (default: active feed
rate)
G85 machines the adjoining cylinder if you position the tool to
diameter X "in front of" the cylinder.
The undercut rounding arcs are executed with the radius 0.6 * I.
Parameters for undercut DIN 509 E
Diameter
I
K
R
<= 18
0.25
2
0.6
> 18 – 80
0.35
2.5
0.6
> 80
0.45
4
1
Parameters for undercut DIN 509 F
Diameter
I
K
R
P
<= 18
0.25
2
0.6
0.1
> 18 – 80
0.35
2.5
0.6
0.2
> 80
0.45
4
1
0.3
 I = undercut depth
 K = undercut width
 R = undercut radius
 P = face depth
 Undercut angle for undercuts according to DIN 509 E and F: 15°
 Transverse angle for an undercut according to DIN 509 F: 8°
316
DIN Programming
 The tool radius compensation is not active.
 Oversizes are not taken into account.
4.21 Undercut cycles
Beispiel: G85
...
N1 T21 G95 F0.23 G96 S248 M3
N2 G0 X62 Z2
N3 G85 X60 Z-30 I0.3
N4 G1 X80
N5 G85 X80 Z-40 K0
N6 G1 X100
N7 G85 X100 Z-60 I1.2 K6 E0.11
N8 G1 X110
...
HEIDENHAIN MANUALplus 620, CNC PILOT 640
317
4.21 Undercut cycles
Undercut according to DIN 509 E with cylinder
machining G851
G851 machines the adjoining cylinder, the undercut, and finishes with
the plane surface. It also machines a cylinder start chamfer when you
enter at least one of the parameters Cut-in length (1st cut length)
or Cut-in radius (1st cut radius).
Parameters
I
Undercut depth (default: value from standard table)
K
Undercut length (default: value from standard table)
W
Undercut angle (default: value from standard table)
R
Undercut radius (default: value from standard table)
B
Cut-in length (1st cut length)—no input: No chamfer machined
at start of cylinder
RB Cut-in radius (1st cut radius)—no input: 1st cut radius is not
machined
WB 1st cut angle (default: 45 °)
E
Reduced feed for machining the undercut (default: active feed
rate)
H
Type of departure (default: 0):
U
 0: Tool returns to the starting point
 1: Tool remains at the end of the plane surface
Grinding oversize for the area of the cylinder (default: 0)
The Steuerung calculates unentered parameters from the diameter of
the cylinder in the standard table (see “Undercut cycle G85” on
page 316).
Blocks following the cycle call
N.. G851 I.. K.. W.. /Cycle call
N.. G0 X.. Z..
N.. G1 Z..
/Corner point of cylinder start chamfer
/Undercut corner
Beispiel: G851
N.. G1 X..
/End point on plane surface
%851.nc
N.. G80
/End of contour definition
[G851]
N1 T2 G95 F0.23 G96 S248 M3
 Undercuts can only be executed in orthogonal, paraxial
contour corners along the longitudinal axis.
 Cutting radius compensation is active.
 Oversizes are not taken into account.
N2 G0 X60 Z2
N3 G851 I3 K15 W30 R2 B5 RB2 WB30 E0.2 H1
N4 G0 X50 Z0
N5 G1 Z-30
N6 G1 X60
N7 G80
END
318
DIN Programming
4.21 Undercut cycles
Undercut according to DIN 509 F with cylinder
machining G852
G852 machines the adjoining cylinder, the undercut, and finishes with
the plane surface. It also machines a cylinder start chamfer when you
enter at least one of the parameters Cut-in length (1st cut length)
or Cut-in radius (1st cut radius).
Parameters
I
Undercut depth (default: value from standard table)
K
Undercut length (default: value from standard table)
W
Undercut angle (default: value from standard table)
R
Undercut radius (default: value from standard table)
P
Face depth (default: value from standard table)
A
Face angle (default: value from standard table)
B
Cut-in length (1st cut length)—no input: No chamfer machined
at start of cylinder
RB Cut-in radius (1st cut radius)—no input: 1st cut radius is not
machined
WB 1st cut angle (default: 45 °)
E
Reduced feed for machining the undercut (default: active feed
rate)
H
Type of departure (default: 0):
U
 0: Tool returns to the starting point
 1: Tool remains at the end of the plane surface
Grinding oversize for the area of the cylinder (default: 0)
The Steuerung calculates unentered parameters automatically from
the diameter in the standard table (see “Undercut cycle G85” on
page 316).
Blocks following the cycle call
N.. G852 I.. K.. W.. /Cycle call
N.. G0 X.. Z..
/Corner point of cylinder start chamfer
N.. G1 Z..
/Undercut corner
N.. G1 X..
/End point on plane surface
N.. G80
/End of contour definition
 Undercuts can only be executed in orthogonal, paraxial
contour corners along the longitudinal axis.
 Cutting radius compensation is active.
 Oversizes are not taken into account.
Beispiel: G852
%852.nc
[G852]
N1 T2 G95 F0.23 G96 S248 M3
N2 G0 X60 Z2
N3 G852 I3 K15 W30 R2 P0.2 A8 B5 RB2 WB30
E0.2 H1
N4 G0 X50 Z0
N5 G1 Z-30
N6 G1 X60
N7 G80
END
HEIDENHAIN MANUALplus 620, CNC PILOT 640
319
4.21 Undercut cycles
Undercut according to DIN 76 with cylinder
machining G853
G853 machines the adjoining cylinder, the undercut, and finishes with
the plane surface. It also machines a cylinder start chamfer when you
enter at least one of the parameters Cut-in length (1st cut length)
or Cut-in radius (1st cut radius).
Parameters
FP
Thread pitch
I
Undercut depth (default: value from standard table)
K
Undercut length (default: value from standard table)
W
Undercut angle (default: value from standard table)
R
Undercut radius (default: value from standard table)
P
Oversize:
B
RB
WB
E
H
 P is not defined: The undercut is machined in one pass
 P is defined: Division into pre-turning and finish-turning
– P = longitudinal oversize; the transverse oversize is preset
to 0.1 mm
Cut-in length (1st cut length)—no input: No chamfer machined
at start of cylinder
Cut-in radius (1st cut radius)—no input: 1st cut radius is not
machined
1st cut angle (default: 45 °)
Reduced feed for machining the undercut (default: active feed
rate)
Type of departure (default: 0):
 0: Tool returns to the starting point
 1: Tool remains at the end of the plane surface
Parameters that are not programmed are automatically calculated by
the Steuerung from the standard table:
 FP from the diameter
 I, K, W, and R from FP (thread pitch)
Blocks following the cycle call
Beispiel: G853
%853.nc
[G853]
N.. G853 FP.. I.. K.. W.. /Cycle call
N1 T2 G95 F0.23 G96 S248 M3
N.. G0 X.. Z..
/Corner point of cylinder start chamfer
N2 G0 X60 Z2
N.. G1 Z..
/Undercut corner
N3 G853 FP1.5 I47 K15 W30 R2 P1 B5 RB2
WB30 E0.2 H1
N.. G1 X..
/End point on plane surface
N.. G80
/End of contour definition
 Undercuts can only be executed in orthogonal, paraxial
contour corners along the longitudinal axis.
 Cutting radius compensation is active.
 Oversizes are not taken into account.
320
N4 G0 X50 Z0
N5 G1 Z-30
N6 G1 X60
N7 G80
END
DIN Programming
4.21 Undercut cycles
Undercut type U G856
G856 machines an undercut and finishes the adjoining plane surface.
A chamfer or rounding (optional) can be machined.
Tool position at the end of the cycle: Cycle start point
Parameters
I
Undercut depth (default: value from standard table)
K
Undercut length (default: value from standard table)
B
Chamfer/rounding:
 B>0: Radius of rounding
 B<0: Width of chamfer
Blocks following the cycle call
N.. G856 I.. K.. /Cycle call
N.. G0 X.. Z..
/Undercut corner
N.. G1 X..
/End point on plane surface
N.. G80
/End of contour definition
Beispiel: G856
%856.nc
[G856]
 Undercuts can only be executed in orthogonal, paraxial
contour corners along the longitudinal axis.
 Cutting radius compensation is active.
 Oversizes are not taken into account.
 If the cutting width of the tool is not defined, the control
assumes that the tool's cutting width equals K.
N1 T3 G95 F0.23 G96 S248 M3
N2 G0 X60 Z2
N3 G856 I47 K7 B1
N4 G0 X50 Z-30
N5 G1 X60
N6 G80
END
HEIDENHAIN MANUALplus 620, CNC PILOT 640
321
4.21 Undercut cycles
Undercut type H G857
G857 machines an undercut. The end point is determined from the
plunge angle in accordance with Undercut type H.
Tool position at the end of the cycle: Cycle start point
Parameters
X
Corner point of contour (diameter)
Z
Corner point of contour
K
Undercut length
R
Radius—no input: No circular element (tool radius = undercut
radius)
W
Plunging angle—no input: W is calculated from K and R
 Undercuts can only be executed in orthogonal, paraxial
contour corners along the longitudinal axis.
 Cutting radius compensation is active.
 Oversizes are not taken into account.
Beispiel: G857
%857.nc
[G857]
N1 T2 G95 F0.23 G96 S248 M3
N2 G0 X60 Z2
N3 G857 X50 Z-30 K7 R2 W30
END
322
DIN Programming
4.21 Undercut cycles
Undercut type K G858
G858 machines an undercut. This cycle performs only one linear cut at
an angle of 45°. The resulting contour geometry therefore depends on
the tool that is used.
Tool position at the end of the cycle: Cycle start point
Parameters
X
Corner point of contour (diameter)
Z
Corner point of contour
I
Undercut depth
 Undercuts can only be executed in orthogonal, paraxial
contour corners along the longitudinal axis.
 Cutting radius compensation is active.
 Oversizes are not taken into account.
Beispiel: G858
%858.nc
[G858]
N1 T9 G95 F0.23 G96 S248 M3
N2 G0 X60 Z2
N3 G858 X50 Z-30 I0.5
END
HEIDENHAIN MANUALplus 620, CNC PILOT 640
323
4.22 Drilling cycles
4.22 Drilling cycles
Overview of drilling and boring cycles and
contour reference
The drilling and boring cycles can be used with driven or stationary
tools.
Drilling and boring cycles:
 G71 Simple drilling: Page 325
 G72 Boring/countersinking (only with contour reference (ID,
NS): Page 327
 G73 Tapping (not with G743 - G746): Page 334
 G74 Deep-hole drilling: Page 331
 G36 Tapping—single path (direct position input): Page 330
 G799 Thread milling (direct position input): Page 338
Pattern definitions:
 G743 Linear pattern on face for drilling and milling cycles: Page 334
 G744 Linear pattern on lateral surface for drilling and milling
cycles: Page 336
 G745 Circular pattern on face for drilling and milling
cycles: Page 335
 G746 Circular pattern on lateral surface for drilling and milling
cycles: Page 337
Possibilities of defining a contour reference:
 Path definition directly in the cycle.
 Reference to a hole or pattern definition in the contour section (ID,
NS) for machining on the front face or lateral surface.
 Centric hole in the turning contour (G49): Page 219
 Pattern definition in the block before the cycle call (G743 - G746)
324
DIN Programming
4.22 Drilling cycles
Drilling cycle G71
G71 is used for axial and radial bore holes using driven or stationary
tools.
Parameters
ID
Drilling contour—Name of the hole definition
NS Block number of contour
XS
ZS
XE
ZE
K
A
V
RB
E
D
BS
BE
H
 Reference to the contour of the hole (G49-Geo, G300-Geo or
G310-Geo)
 No input: Single hole without contour description
Starting point of radial hole (diameter value)
Starting point of axial hole
End point of radial hole (diameter value)
End point of axial hole
Boring depth (hole depth) (alternative to XE/ZE)
Drilling lengths (default: 0)
Bore (through-drilling) variant (feed rate reduction 50%)—
(default: 0)
 0: No feed rate reduction
 1: Feed reduction for through-drilling
 2: Feed reduction for pre-drilling
 3: Feed reduction for pre-drilling and through-drilling
Retraction plane (radial holes, holes in the YZ plane:
diameter)—(default: return to the starting position or to the
safety clearance)
Period of dwell for chip breaking at end of hole (in seconds)—
(default: 0)
Retraction type (default: 0)
 0: Rapid traverse
 1: Feed rate
Start element no. (number of the first hole to be machined in a
pattern)
End element no. (number of the last hole to be machined in a
pattern)
(Spindle) Brake off (default: 0)
 0: Spindle brake on
 1: Spindle brake off
Beispiel: G71
...
N1 T5 G97 S1000 G95 F0.2 M3
N2 G0 X0 Z5
N3 G71 Z-25 A5 V2 [drilling]
...
 Single hole without contour description: Program XS or
ZS as alternative.
 Hole with contour description: Do not program XS, ZS.
 Hole pattern: NS refers to the hole contour, and not the
definition of the pattern.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
325
4.22 Drilling cycles
Parameter combinations for single holes without contour
description
XS, XE
ZS, ZE
XS, K
ZS, K
XE, K
ZE, K
Feed rate reduction:
 Indexable insert drill and twist drill with 180° drilling angle
 A feed rate reduction is only effective if the parameter "Drilling
length A" has been defined.
 Other drills
 Beginning of hole: Feed rate reduction as programmed in V
 End of hole: Reduction as of hole end point – length of first cut –
safety clearance
 Length of first cut = tool tip
 Safety clearance: See user parameter or G47, G147
Cycle run
1  Hole without contour description: Tool is located at the
starting point (safety distance from the bore hole).
 Hole with contour description: Tool moves at rapid traverse
to the starting point:
 RB not programmed: Moves up to the safety clearance
 RB programmed: Moves to the position RB and then to the
safety clearance
2 Spot drilling. Feed rate reduction depending on V
3 Drilling at feed rate.
4 Through drilling. Feed rate reduction depending on V
5 Retraction at rapid traverse or feed rate, depending on D.
6 Retraction position:
 RB not programmed: Retraction to the starting point
 RB programmed: Retraction to the position RB
326
DIN Programming
4.22 Drilling cycles
Boring, countersinking G72
G72 is used for holes with contour definition (individual hole or hole
pattern). Use G72 for the following axial and radial drilling functions
using driven or stationary tools:
 Boring
 Countersinking
 Reaming
 NC drilling
 Centering
Parameters
ID
Drilling contour—Name of the hole definition
NS Block number of contour. Reference to the contour of the hole
(G49-Geo, G300-Geo or G310-Geo)
RB Retraction plane (radial holes, holes in the YZ plane:
diameter)—(default: return to the starting position or to the
safety clearance)
E
Period of dwell for chip breaking at end of hole (in seconds)—
(default: 0)
D
Retraction type (default: 0)
BS
BE
H
 0: Rapid traverse
 1: Feed rate
Start element no. (number of the first hole to be machined in a
pattern)
End element no. (number of the last hole to be machined in a
pattern)
(Spindle) Brake off (default: 0)
 0: Spindle brake on
 1: Spindle brake off
Cycle run
1 Moves to the starting point at rapid traverse, depending on RB:
2
3
4
5
 RB not programmed: Moves up to the safety clearance
 RB programmed: Moves to the position RB and then to the
safety clearance
Drills at reduced feed rate (50%).
Moves at feed rate to end of hole.
Retraction at rapid traverse or feed rate, depending on D.
Return position depends on RB:
 RB not programmed: Retraction to the starting point
 RB programmed: Retraction to the position RB
Hole pattern: NS refers to the hole contour, and not the
definition of the pattern.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
327
4.22 Drilling cycles
Tapping G73
G73 cuts axial/radial threads using driven or stationary tools.
Parameters
ID
Drilling contour—Name of the hole definition
NS
Block number of contour
ZS
 Reference to the contour of the hole (G49-Geo, G300-Geo or
G310-Geo)
 No input: Single hole without contour description
Starting point of radial hole (diameter value)—single hole
without contour description
Starting point of axial hole
XE
Single hole without contour description
End point of radial hole (diameter value)
ZE
Single hole without contour description
End point of axial hole
K
Single hole without contour description
Boring depth (hole depth) (alternative to XE/ZE)
XS
F
B
S
J
RB
P
I
BS
BE
H
Single hole without contour description
Thread pitch (prevails over the contour description)
Run-in length
Retraction speed (default: Shaft speed for tapping)
Retraction length when using floating tap holders (default: 0)
Retraction plane (radial holes: diameter)—(default: return to
the starting position or to the safety clearance)
Chip breaking depth
Retraction distance
Start element no. (number of the first hole to be machined in a
pattern)
End element no. (number of the last hole to be machined in a
pattern)
(Spindle) Brake off (default: 0)
 0: Spindle brake on
 1: Spindle brake off
The starting position is calculated from the safety clearance and the
run-in (slope) length B.
328
DIN Programming
4.22 Drilling cycles
Parameter combinations for single holes without contour
description
XS, XE
ZS, ZE
XS, K
ZS, K
XE, K
ZE, K
Retraction length J: Use this parameter for floating tap holders. The
cycle calculates a new nominal pitch on the basis of the thread depth,
the programmed pitch, and the "retraction length." The nominal pitch
is somewhat smaller than the pitch of the tap. During tapping, the tap
is pulled away from the chuck by the retraction length. With this
method you can achieve higher service life from the taps.
 Hole pattern: NS refers to the hole contour, and not the
definition of the pattern.
 Single hole without contour description: Program XS or
ZS as alternative.
 Hole with contour description: Do not program XS, ZS.
 Cycle stop interrupts the tapping operation.
 Cycle start resumes the tapping operation.
 Use the feed rate override function for speed changes.
 Spindle override is not effective.
 Use a floating tap holder if the driven tool is not
controlled, e.g. by a ROD encoder.
Cycle run
1 Moves at rapid traverse to the starting point:
2
3
4
 RB not programmed: Moves directly to the starting point
 RB programmed: Moves to the position RB and then to the
starting point
Moves along run-in length B at feed rate (synchronization of
spindle and feed drives).
Cuts the thread.
Retracts with return speed S:
 RB not programmed: To the starting point
 RB programmed: To the position RB
HEIDENHAIN MANUALplus 620, CNC PILOT 640
329
4.22 Drilling cycles
Tapping G36—Single path
G36 cuts axial/radial threads using driven or stationary tools.
Depending on X/Z, G36 decides whether a radial or axial hole will be
machined.
Move to the starting point before G36. G36 returns to the starting
position after having cut the thread.
Parameters
X
End point of radial hole (diameter value)
Z
End point of axial hole
F
Feed per revolution (thread pitch)
B
Run-in length for synchronizing spindle and feed drive
S
Retraction speed (default: Shaft speed for tapping)
P
Chip breaking depth
I
Retraction distance
Type of taps:
 Stationary tap: Main spindle and feed drive are synchronized.
 Driven tap: Driven tool and feed drive are synchronized.
 Cycle stop interrupts the tapping operation.
 Cycle start resumes the tapping operation.
 Use the feed rate override function for speed changes.
 Spindle override is not effective.
 Use a floating tap holder if the driven tool is not
controlled, e.g. by a ROD encoder.
Beispiel: G36
...
N1 T5 G97 S1000 G95 F0.2 M3
N2 G0 X0 Z5
N3 G71 Z-30
N4 G14 Q0
N5 T6 G97 S600 M3
N6 G0 X0 Z8
N7 G36 Z-25 F1.5 B3 [tapping]
...
330
DIN Programming
4.22 Drilling cycles
Deep-hole drilling G74
G74 is used for axial and radial holes in several stages using driven or
stationary tools.
Parameters
ID
Drilling contour—Name of the hole definition
NS Block number of contour
XS
ZS
XE
ZE
K
P
I
B
J
R
A
V
RB
E
D
BS
BE
H
 Reference to the contour of the hole (G49-Geo, G300-Geo or
G310-Geo)
 No input: Single hole without contour description
Starting point of radial hole (diameter value)
Starting point of axial hole
End point of radial hole (diameter value)
End point of axial hole
Boring depth (hole depth) (alternative to XE/ZE)
First hole depth
Reduction value (default: 0)
Retraction distance (default: to starting point of hole)
Minimum hole depth (default: 1/10 of P)
Safety distance (inside)
Drilling lengths—(default: 0)
Bore (through-drilling) variant (feed rate reduction 50%)—
(default: 0)
 0: No feed rate reduction
 1: Feed reduction for through-drilling
 2: Feed reduction for pre-drilling
 3: Feed reduction for pre-drilling and through-drilling
Retraction plane (radial holes: diameter)—(default: return to
the starting position or to the safety clearance)
Period of dwell for chip breaking at end of hole (in seconds)—
(default: 0)
Retraction speed and infeed within the hole (default: 0)
 0: Rapid traverse
 1: Feed rate
Start element no. (number of the first hole to be machined in a
pattern)
End element no. (number of the last hole to be machined in a
pattern)
(Spindle) Brake off (default: 0)
 0: Spindle brake on
 1: Spindle brake off
Beispiel: G74
...
N1 M5
N2 T4 G197 S1000 G195 F0.2 M103
N3 M14
N4 G110 C0
N5 G0 X80 Z2
N6 G745 XK0 YK0 Z2 K80 Wi90 Q4 V2
N7 G74 Z-40 R2 P12 I2 B0 J8 [drilling]
N8 M15
...
HEIDENHAIN MANUALplus 620, CNC PILOT 640
331
4.22 Drilling cycles
Parameter combinations for single holes without contour
description
XS, XE
ZS, ZE
XS, K
ZS, K
XE, K
ZE, K
The cycle is used for:
 Single hole without contour description
 Hole with contour description (single hole or hole pattern)
"1st hole depth P" is used for the first pass. The control then
automatically reduces the drilling depth with each subsequent pass by
the reduction value I, however, without falling below the minimum
drilling depth J. After each pass, the tool is retracted either by
retraction distance B or to the starting point of the hole. If the safety
distance R is defined, the tool is positioned to this distance at rapid
traverse inside the hole.
Feed rate reduction:
 Indexable insert drill and twist drill with 180° drilling angle
 A feed rate reduction is only effective if the parameter "Drilling
length A" has been defined.
 Other drills
 Beginning of hole: Feed rate reduction as programmed in V
 End of hole: Reduction as of hole end point – length of first cut –
safety clearance
 Length of first cut = tool tip
 Safety clearance: See user parameter or G47, G147
 Single hole without contour description: Program XS or
ZS as alternative.
 Hole with contour description: Do not program XS, ZS.
 Hole pattern: NS refers to the hole contour, and not the
definition of the pattern.
 A "feed rate reduction at end" goes into effect only at the
last drilling stage.
332
DIN Programming
4.22 Drilling cycles
Cycle run
1  Hole without contour description: Tool is located at the
starting point (safety distance from the bore hole).
 Hole with contour description:: Tool moves at rapid traverse
to the starting point:
 RB not programmed: Moves up to the safety clearance
 RB programmed: Moves to the position RB and then to the
safety clearance
2 Spot drilling. Feed rate reduction depending on V
3 Drills the hole in several passes
4 Through drilling. Feed rate reduction depending on V
5 Retraction at rapid traverse or feed rate, depending on D.
6 Return position depends on RB:
 RB not programmed: Retraction to the starting point
 RB programmed: Retraction to the position RB
HEIDENHAIN MANUALplus 620, CNC PILOT 640
333
4.22 Drilling cycles
Linear pattern, face G743
Cycle G743 is used to machine linear drilling or milling patterns in
which the individual features are arranged at a regular spacing on the
face.
If the Final point ZE has not been defined, the drilling/milling cycle
of the next NC block is used as a reference. Using this principle, you
can combine pattern definitions with
 Drilling cycles (G71, G74, G36)
 The milling cycle for a linear slot (G791)
 The contour milling cycle with "free contour" (G793)
Parameters
XK
Starting point of pattern in Cartesian coordinates
YK
Starting point of pattern in Cartesian coordinates
ZS
Starting point of drilling/milling operation
ZE
Final point of drilling/milling operation
X
Diameter (starting point of pattern in polar coordinates)
C
Angle (starting point of pattern in polar coordinates)
A
Pattern angle
I
Final point of pattern (Cartesian)
Ii
(Final point) Pattern distance (Cartesian)
J
Final point of pattern (Cartesian)
Ji
(Final point) Pattern distance (Cartesian)
R
Length (distance between first and last position)
Ri
Length (distance to next position)
Q
Number of holes/figures—(default: 1)
Beispiel: G743
%743.nc
[G743]
N1 T7 G197 S1200 G195 F0.2 M104
N2 M14
N3 G110 C0
N4 G0 X100 Z2
N5 G743 XK20 YK5 A45 Ri30 Q2
N6 G791 X50 C0 ZS0 ZE-5 P2 F0.15
Parameter combinations for defining the starting point and the
pattern positions:
 Starting point of pattern:
 XK, YK
 X, C
 Pattern positions:
 I, J and Q
 Ii, Ji and Q
 R, A and Q
 Ri, Ai and Q
N7 M15
END
Beispiel: Sequence of commands
[Simple drilling pattern]
N.. G743 XK.. YK.. ZS.. ZE.. I.. J.. Q..
...
[Drilling pattern with deep-hole drilling]
N.. G743 XK.. YK.. ZS.. I.. J.. Q..
N.. G74 ZE.. P.. I..
...
[Milling pattern with linear slot]
N.. G743 XK.. YK.. ZS.. I.. J.. Q..
N.. G791 K.. A.. Z..
...
334
DIN Programming
4.22 Drilling cycles
Circular pattern, face G745
Cycle G745 is used to machine drilling or milling patterns in which the
individual features are arranged at a regular spacing in a circle or
circular arc on the face.
If the Final point ZE has not been defined, the drilling/milling cycle
of the next NC block is used as a reference. Using this principle, you
can combine pattern definitions with
 Drilling cycles (G71, G74, G36)
 The milling cycle for a linear slot (G791)
 The contour milling cycle with "free contour" (G793)
Parameters
XK
Center of pattern in Cartesian coordinates
YK
Center of pattern in Cartesian coordinates
ZS
Starting point of drilling/milling operation
ZE
Final point of drilling/milling operation
X
Diameter (center point of pattern in polar coordinates)
C
Angle (center point of pattern in polar coordinates)
A
Starting angle (position of first hole/figure)
W
Final angle (position of last hole/figure)
Wi
Final angle (distance to the next position)
Q
Number of holes/figures—(default: 1)
V
Rotation direction (default: 0)
 V=0, without W: Figures are arranged on a full circle
 V=0, with W: Figures are arranged on the longer circular arc
 V=0, with Wi: The algebraic sign of Wi defines the direction
(Wi<0: clockwise)
 V=1, with W: Clockwise
 V=1, with Wi: Clockwise (algebraic sign of Wi has no effect)
 V=2, with W: Counterclockwise
 V=2, with Wi: Counterclockwise (algebraic sign of Wi has no
effect)
Beispiel: G745
%745.nc
[G745]
N1 T7 G197 S1200 G195 F0.2 M104
N2 M14
N3 G110 C0
N4 G0 X100 Z2
N5 G745 XK0 YK0 K50 A0 Q3
N6 G791 K30 A0 ZS0 ZE-5 P2 F0.15
N7 M15
END
Beispiel: Sequence of commands
[Simple drilling pattern]
Parameter combinations for defining the center of the pattern and
the pattern positions:
N.. G745 XK.. YK.. ZS.. ZE.. A.. W.. Q..
 Center of pattern:
 X, C
 XK, YK
[Drilling pattern with deep-hole drilling]
 Pattern positions:
 A, W and Q
 A, Wi and Q
...
N.. G745 XK.. YK.. ZS.. A.. W.. Q..
N.. G74 ZE.. P.. I..
...
[Milling pattern with linear slot]
N.. G745 XK.. YK.. ZS.. ZE.. A.. W.. Q..
N.. G791 K.. A.. Z..
...
HEIDENHAIN MANUALplus 620, CNC PILOT 640
335
4.22 Drilling cycles
Linear pattern, lateral surface G744
Cycle G744 is used to machine linear drilling patterns or milling
patterns in which the individual features are arranged at a regular
spacing on the lateral surface.
Parameter combinations for defining the starting point and the
pattern positions:
 Starting point of pattern: Z, C
 Pattern positions:
 W and Q
 Wi and Q
If the Final point XE has not been defined, the drilling/milling cycle
or the figure definition of the next NC block is used as a reference.
Using this principle, you can combine pattern definitions with drilling
cycles (G71, G74, G36) or milling cycles (figure definitions with G314,
G315, G317).
Parameters
XS
Starting point of drilling/milling operation (diameter value)
Z
Starting point of pattern in polar coordinates
XE
Final point of drilling/milling operation (diameter value)
ZE
Final point of pattern (default: Z)
C
Starting angle of pattern in polar coordinates
W
Final angle of pattern—no input: Holes/figures are arranged on
the lateral surface at regular spacing
Wi
Final angle (angle increment), distance to the next position
Q
Number of holes/figures—(default: 1)
A
Angle (orientation angle of the pattern)
R
Length (distance between first and last position [mm],
reference: unrolled lateral surface XS)
Ri
Length (distance from the next position [mm], reference:
unrolled lateral surface XS)
Beispiel: G744
%744.nc
[G744]
N1 T6 G197 S1200 G195 F0.2 M104
N2 M14
N3 G110 C0
N4 G0 X110 Z2
N5 G744 XS102 Z-10 ZE-35 C0 W270 Q5
N6 G71 XS102 K7
N7 M15
END
Beispiel: Sequence of commands
[Simple drilling pattern]
N.. G744 Z.. C.. XS.. XE.. ZE.. W.. Q..
...
[Drilling pattern with deep-hole drilling]
N.. G744 Z.. C.. XS.. XE.. ZE.. W.. Q..
N.. G74 XE.. P.. I..
...
[Milling pattern with linear slot]
N.. G744 Z.. C.. XS.. XE.. ZE.. W.. Q..
N.. G792 K.. A.. XS..
...
336
DIN Programming
4.22 Drilling cycles
Circular pattern, lateral surface G746
Cycle G746 is used to machine drilling patterns or milling patterns in
which the individual features are arranged at a regular spacing in a
circle or circular arc on the lateral surface.
Parameter combinations for defining the center of the pattern and the
pattern positions:
 Center of pattern: Z, C
 Pattern positions:
 W and Q
 Wi and Q
If the Final point XE has not been defined, the drilling/milling cycle
or the figure definition of the next NC block is used as a reference.
Using this principle, you can combine pattern definitions with drilling
cycles (G71, G74, G36) or milling cycles (figure definitions with G314,
G315, G317).
Parameters
Z
Center of pattern in polar coordinates
C
Angle (center point of pattern in polar coordinates)
XS
Starting point of drilling/milling operation (diameter value)
XE
Final point of drilling/milling operation (diameter value)
K
(Pattern) diameter
A
Starting angle (position of first hole/figure)
W
Final angle (position of last hole/figure)
Wi
Final angle (angle increment), distance to the next position
Q
Number of holes/figures—(default: 1)
V
Rotation direction (default: 0)
 V=0, without W: Figures are arranged on a full circle
 V=0, with W: Figures are arranged on the longer circular arc
 V=0, with Wi: The algebraic sign of Wi defines the direction
(Wi<0: clockwise)
 V=1, with W: Clockwise
 V=1, with Wi: Clockwise (algebraic sign of Wi has no effect)
 V=2, with W: Counterclockwise
 V=2, with Wi: Counterclockwise (algebraic sign of Wi has no
effect)
Beispiel: G746
%746.nc
[G746]
N1 T6 G197 S1200 G195 F0.2 M104
N2 M14
N3 G110 C0
N4 G0 X110 Z2
N5 G746 Z-40 C0 K40 Q8
N6 G71 XS102 K7
N7 M15
END
Beispiel: Sequence of commands
[Simple drilling pattern]
N.. G746 Z.. C.. XS.. XE.. K.. A.. W.. Q..
...
[Drilling pattern with deep-hole drilling]
N.. G746 Z.. C.. XS.. K.. A.. W.. Q..
N.. G74 XE.. P.. I..
...
[Milling pattern with linear slot]
N.. G746 Z.. C.. XS.. K.. A.. W.. Q..
N.. G792 K.. A.. XS..
...
HEIDENHAIN MANUALplus 620, CNC PILOT 640
337
4.22 Drilling cycles
Thread milling, axial G799
G799 mills a thread in existing holes.
Place the tool on the center of the hole before calling G799. The cycle
positions the tool on the end point of the thread within the hole. Then
the tool approaches on "approaching radius R" and mills the thread.
During this, the tool advances by the thread pitch F. Following that, the
cycle retracts the tool and returns it to the starting point. With
parameter V, you can program whether the thread is to be milled in
one rotation or, with single-point tools, in several rotations.
Parameters
I
Thread diameter
Z
Starting point Z
K
Thread depth
R
Approach radius
F
Thread pitch
J
Direction of thread (default: 0)
H
 0: Right-hand thread
 1: Left-hand thread
Cutting direction (default: 0)
V
 0: Up-cut milling
 1: Climb milling
Milling method
 0: The thread is milled in a 360-degree helix
 1: The thread is milled in several helical paths (single-point
tool)
Use thread-milling tools for cycle G799.
Beispiel: G799
%799.nc
Danger of collision!
[G799]
Be sure to consider the hole diameter and the diameter of
the milling cutter when programming "approach radius R."
N1 T9 G195 F0.2 G197 S800
N2 G0 X100 Z2
N3 M14
N4 G110 Z2 C45 X100
N5 G799 I12 Z0 K-20 F2 J0 H0
N6 M15
END
338
DIN Programming
4.23 C-axis commands
4.23 C-axis commands
Reference diameter G120
G120 determines the reference diameter of the unrolled lateral
surface. Program G120 if you use CY for G110 to G113. G120 is a
modal function.
Parameters
X
Diameter
Beispiel: G120
...
N1 T7 G197 S1200 G195 F0.2 M104
N2 M14
N3 G120 X100 [reference diameter]
N4 G110 C0
N5 G0 X110 Z5
N6 G41 Q2 H0
N7 G110 Z-20 CY0
N8 G111 Z-40
N9 G113 CY39.2699 K-40 J19.635
N10 G111 Z-20
N11 G113 CY0 K-20 J19.635
N12 G40
N13 G110 X105
N14 M15
...
Zero point shift, C axis G152
G152 defines an absolute zero point for the C axis (reference:
reference point, C axis). The zero point is valid until the end of the
program.
Parameters
C
Angle: Spindle position of the new C-axis zero point
Beispiel: G152
...
N1 M5
N2 T7 G197 S1010 G193 F0.08 M104
N3 M14
N4 G152 C30 [zero point of C axis]
N5 G110 C0
N6 G0 X122 Z-50
N7 G71 X100
N8 M15
...
HEIDENHAIN MANUALplus 620, CNC PILOT 640
339
4.23 C-axis commands
Standardize C axis G153
G153 resets a traverse angle >360° or <0° to the corresponding angle
modulo 360°—without moving the C axis.
G153 is only used for lateral-surface machining. An
automatic modulo 360° function is carried out on the face.
340
DIN Programming
4.24 Front/rear-face machining
4.24 Front/rear-face machining
Rapid traverse on front/rear face G100
G100 moves at rapid traverse along the shortest path to the end point.
Parameters
X
End point (diameter)
C
End angle—for angle direction, see graphic support window
XK
End point (Cartesian)
YK
End point (Cartesian)
Z
End point (default: current Z position)
Programming:
 X, C, XK, YK, Z: Absolute, incremental or modal
 Program either X–C or XK–YK
Danger of collision!
During G100 the tool moves on a linear path. To position
the workpiece to a defined angle, use G110.
Beispiel: G100
...
N1 T7 G197 S1200 G195 F0.2 M104
N2 M14
N3 G110 C0
N4 G0 X100 Z2
N6 G100 XK20 YK5 [rapid traverse on face]
N7 G101 XK50
N8 G103 XK5 YK50 R50
N9 G101 XK5 YK20
N10 G102 XK20 YK5 R20
N11 G14
N12 M15
...
HEIDENHAIN MANUALplus 620, CNC PILOT 640
341
4.24 Front/rear-face machining
Line segment on front/rear face G101
G101 moves the tool on a linear path at the feed rate to the "end point."
Parameters
X
End point (diameter)
C
End angle—for angle direction, see graphic support window
XK
End point (Cartesian)
YK
End point (Cartesian)
Z
End point (default: current Z position)
Parameters for contour description (G80)
AN Angle to positive XK axis
BR Chamfer/rounding. Defines the transition to the next contour
element. When entering a chamfer/rounding, program the
theoretical end point.
Q
 No input: Tangential transition
 BR=0: No tangential transition
 BR>0: Radius of rounding
 BR<0: Width of chamfer
Point of intersection. End point if the line segment intersects a
circular arc (default: 0):
 Q=0: Near point of intersection
 Q=1: Far point of intersection
Beispiel: G101
...
N1 T70 G197 S1200 G195 F0.2 M104
N2 M14
N3 G110 C0
N4 G0 X110 Z2
Programming:
N5 G100 XK50 YK0
 X, C, XK, YK, Z: Absolute, incremental or modal
 Program either X–C or XK–YK
N6 G1 Z-5
N7 G42 Q1
N8 G101 XK40 [linear path on face]
Using the parameters AN, BR and Q is only allowed if the
contour description is concluded by G80 and used for a
cycle.
N9 G101 YK30
N10 G103 XK30 YK40 R10
N11 G101 XK-30
N12 G103 XK-40 YK30 R10
N13 G101 YK-30
N14 G103 XK-30 YK-40 R10
N15 G101 XK30
N16 G103 XK40 YK-30 R10
N17 G101 YK0
N18 G100 XK110 G40
N19 G0 X120 Z50
N20 M15
...
342
DIN Programming
4.24 Front/rear-face machining
Circular arc on front/rear face G102/G103
G102/G103 moves the tool in a circular arc at the feed rate to the "end
point." The direction of rotation is shown in the graphic support
window.
Parameters
X
End point (diameter)
C
End angle—for angle direction, see graphic support window
XK
End point (Cartesian)
YK
End point (Cartesian)
R
Radius
I
Center point (Cartesian)
J
Center point (Cartesian)
K
Center point for H=2, 3 (Z direction)
Z
End point (default: current Z position)
H
Circular plane (working plane)—(default: 0)
 H=0, 1: Machining in XY plane (front face)
 H=2: Machining in YZ plane
 H=3: Machining in XZ plane
Parameters for contour description (G80)
AN Angle to positive XK axis
BR Chamfer/rounding. Defines the transition to the next contour
element. When entering a chamfer/rounding, program the
theoretical end point.
Q
 No input: Tangential transition
 BR=0: No tangential transition
 BR>0: Radius of rounding
 BR<0: Width of chamfer
Point of intersection. End point if the line segment intersects a
circular arc (default: 0):
 Q=0: Near point of intersection
 Q=1: Far point of intersection
Beispiel: G102, G103
...
N1 T7 G197 S1200 G195 F0.2 M104
N2 M14
Using the parameters AN, BR and Q is only allowed if the
contour description is concluded by G80 and used for a
cycle.
N3 G110 C0
N4 G0 X100 Z2
N6 G100 XK20 YK5
N7 G101 XK50
N8 G103 XK5 YK50 R50 [circular arc]
N9 G101 XK5 YK20
N10 G102 XK20 YK5 R20
N12 M15
...
HEIDENHAIN MANUALplus 620, CNC PILOT 640
343
4.24 Front/rear-face machining
If you program H=2 or H=3, you can machine linear slots with a
circular base. If
 H=2: Define the circle center with I and K.
 H=3: Define the circle center with J and K.
Programming:
 X, C, XK, YK, Z: Absolute, incremental or modal
 I, J, K: Absolute or incremental
 Program either X–C or XK–YK
 Program either center or radius
 For radius: Only arcs <= 180° are possible
 End point in the coordinate origin: Program XK=0 and
YK=0.
344
DIN Programming
4.25 Lateral surface machining
4.25 Lateral surface machining
Rapid traverse, lateral surface G110
G110 moves at rapid traverse along the shortest path to the end point.
G110 is recommended for positioning the C axis to a defined angle
(programming: N.. G110 C...).
Parameters
Z
End point
C
End angle
CY
End point as linear value (reference: unrolled reference
diameter G120)
X
End point (diameter)
Programming:
 Z, C, CY: Absolute, incremental, or modal
 Program either Z–C or Z–CY
Beispiel: G110
...
N1 T8 G197 S1200 G195 F0.2 M104
N2 M14
N3 G120 X100
N4 G110 C0 [rapid, lateral surface]
N5 G0 X110 Z5
N6 G110 Z-20 CY0
N7 G111 Z-40
N8 G113 CY39.2699 K-40 J19.635
N9 G111 Z-20
N10 G113 CY0 K-20 J19.635
N11 M15
...
HEIDENHAIN MANUALplus 620, CNC PILOT 640
345
4.25 Lateral surface machining
Line segment on lateral surface G111
G111 moves the tool on a linear path at the feed rate to the "end point."
Parameters
Z
End point
C
End angle—for angle direction, see graphic support window
CY
End point as linear value (reference: unrolled reference
diameter G120)
X
End point (diameter value)—(default: current X position)
Parameters for contour description (G80)
AN Angle to positive Z axis
BR Chamfer/rounding. Defines the transition to the next contour
element. When entering a chamfer/rounding, program the
theoretical end point.
Q
 No input: Tangential transition
 BR=0: No tangential transition
 BR>0: Radius of rounding
 BR<0: Width of chamfer
Point of intersection. End point if the line segment intersects a
circular arc (default: 0):
 Q=0: Near point of intersection
 Q=1: Far point of intersection
Using the parameters AN, BR and Q is only allowed if the
contour description is concluded by G80 and used for a
cycle.
Beispiel: G111
...
[G111, G120]
N1 T8 G197 S1200 G195 F0.2 M104
N2 M14
N3 G120 X100
N4 G110 C0
N5 G0 X110 Z5
N6 G41 Q2 H0
N7 G110 Z-20 CY0
Programming:
 Z, C, CY: Absolute, incremental, or modal
 Program either Z–C or Z–CY
N8 G111 Z-40 [linear path on lateral surface]
N9 G113 CY39.2699 K-40 J19.635
N10 G111 Z-20
N11 G113 CY0 K-20 J19.635
N12 G40
N13 G110 X105
N14 M15
...
346
DIN Programming
4.25 Lateral surface machining
Circular arc on lateral surface G112/G113
G112/G113 moves the tool in a circular arc at the feed rate to the "end
point."
Parameters
Z
End point
C
End angle—for angle direction, see graphic support window
CY
End point as linear value (reference: unrolled reference
diameter G120)
R
Radius
K
Center
J
Center point as linear value (referenced to unrolled G120
reference diameter)
W
Center of angle (for angle direction, see graphic support
window)
X
End point (diameter value)—(default: current X position)
Parameters for contour description (G80)
AN Angle to positive Z axis
BR Chamfer/rounding. Defines the transition to the next contour
element. When entering a chamfer/rounding, program the
theoretical end point.
Q
 No input: Tangential transition
 BR=0: No tangential transition
 BR>0: Radius of rounding
 BR<0: Width of chamfer
Point of intersection. End point if the line segment intersects a
circular arc (default: 0):
 Q=0: Near point of intersection
 Q=1: Far point of intersection
Beispiel: G112, G113
Using the parameters AN, BR and Q is only allowed if the
contour description is concluded by G80 and used for a
cycle.
...
N1 T8 G197 S1200 G195 F0.2 M104
N2 M14
Programming:
N3 G120 X100
 Z, C, CY: Absolute, incremental, or modal
 K, W, J: Absolute or incremental
 Program either Z–C or Z–CY and K–J
 Program either center or radius
 For radius: Only arcs <= 180° are possible
N4 G110 C0
N5 G0 X110 Z5
N7 G110 Z-20 CY0
N8 G111 Z-40
N9 G113 CY39.2699 K-40 J19.635 [circular arc]
N10 G111 Z-20
N11 G112 CY0 K-20 J19.635
N13 M15
HEIDENHAIN MANUALplus 620, CNC PILOT 640
347
4.26 Milling cycles
4.26 Milling cycles
Overview of milling cycles
 G791 Linear slot on the face. The position and length of the slot are
defined directly in the cycle; slot width = cutter diameter: Page 349
 G792 Linear slot on the lateral surface. The position and length of
the slot are defined directly in the cycle; slot width = cutter
diameter: Page 350
 G793 Contour and figure milling cycle on the face. The contour is
described directly after the cycle and concluded by G80
(compatibility cycle MANUALplus 4110): Page 351
 G794 Contour and figure milling cycle on the lateral surface. The
contour is described directly after the cycle and concluded by G80
(compatibility cycle MANUALplus 4110): Page 353
 G797 Face milling. Mills figures (circles, polygons, individual
surfaces, contours) as islands on the face: Page 355
 G798 Helical slot milling. Mills a helical slot on the lateral surface;
slot width = cutter diameter: Page 357
 G840 Contour milling. Mills ICP contours and figures. Closed
contours are machined inside/outside of the contour, or on the
contour. Open contours are machined from the left/right of the
contour, or on the contour. G840 is used on the face and lateral
surface: Page 358
 G845 Pocket milling—roughing. Roughs out closed ICP contours
and figures on the face and lateral surface: Page 368
 G846 Pocket milling—finishing. Finishes closed ICP contours and
figures on the face and lateral surface: Page 374
Contour definitions in the MACHINING section (figures)
 Face
 G301 Linear slot: Page 234
 G302/G303 Circular slot: Page 234
 G304 Full circle: Page 235
 G305 Rectangle: Page 235
 G307 Eccentric polygon: Page 236
 Lateral surface
 G311 Linear slot: Page 243
 G312/G313 Circular slot: Page 243
 G314 Full circle: Page 244
 G315 Rectangle: Page 244
 G317 Eccentric polygon: Page 245
348
DIN Programming
4.26 Milling cycles
Linear slot on face G791
G791 mills a slot from the current tool position to the end point. The
slot width equals the diameter of the milling cutter. Oversizes are not
taken into account.
Parameters
X
Final point of slot in polar coordinates (diameter)
C
Final angle. Final point of slot in polar coordinates (for angle
direction, see help graphic)
XK
Final point of slot (Cartesian)
YK
Final point of slot (Cartesian)
K
Slot length referenced to center of cutter
A
Slot angle (reference: see help graphic)
ZE
Milling floor
ZS
Milling top edge
J
Milling depth
P
F
 J>0: Infeed direction –Z
 J<0: Infeed direction +Z
Maximum approach (default: total depth in one infeed)
Approach feed (infeed rate) (default: active feed rate)
Parameter combinations for definition of the end point: see help
graphic
Parameter combinations for definition of the milling plane:
 Milling floor ZE, milling top edge ZS
 Milling floor ZE, milling depth J
 Milling top edge ZS, milling depth J
 Milling floor ZE
 Rotate the spindle to the desired angle position before
calling G791.
 If you use a spindle positioning device (no C axis), an
axial slot is machined centrically to the rotary axis.
 If J or ZS is defined, the tool approaches to safety
clearance in Z and then mills the slot. If J and ZS are not
defined, the milling cycle starts from the current tool
position.
Beispiel: G791
%791.nc
[G791]
N1 T7 G197 S1200 G195 F0.2 M104
N2 M14
N3 G110 C0
N4 G0 X100 Z2
N5 G100 XK20 YK5
N6 G791 XK30 YK5 ZE-5 J5 P2
N7 M15
END
HEIDENHAIN MANUALplus 620, CNC PILOT 640
349
4.26 Milling cycles
Linear slot on lateral surface G792
G792 mills a slot from the current tool position to the end point. The
slot width equals the diameter of the milling cutter. Oversizes are not
taken into account.
Parameters
Z
Final point of slot
C
Final angle. Final point of slot (for angle direction, see help
graphic)
K
Slot length referenced to center of cutter
A
Slot angle (reference: see help graphic)
XE
Milling floor
XS
Milling top edge
J
Milling depth
P
F
 J>0: Infeed direction –X
 J<0: Infeed direction +X
Maximum approach (default: total depth in one infeed)
Approach feed (infeed rate) (default: active feed rate)
Parameter combinations for definition of the end point: see help
graphic
Parameter combinations for definition of the milling plane:
 Milling floor XE, milling top edge XS
 Milling floor XE, milling depth J
 Milling top edge XS, milling depth J
 Milling floor XE
 Rotate the spindle to the desired angle position before
calling G792.
 If you use a spindle positioning device (no C axis), a
radial slot is machined parallel to the Z axis.
 If J or XS is defined, the tool approaches to safety
clearance in X and then mills the slot. If J and XS are not
defined, the milling cycle starts from the current tool
position.
Beispiel: G792
%792.nc
[G792]
N1 T8 G197 S1200 G195 F0.2 M104
N2 M14
N3 G110 C0
N4 G0 X110 Z5
N5 G0 X102 Z-30
N6 G792 K25 A45 XE97 J3 P2 F0.15
N7 M15
END
350
DIN Programming
4.26 Milling cycles
Contour and figure milling cycle, face G793
G793 mills figures or (open or closed) "free" contours.
G793 is followed by:
 The figure to be milled with:
 Contour definition of the figure (G301 to G307)—See "Front and
rear face contours" on page 230.
 Conclusion of milling contour (G80)
 The free contour with:
 Starting point of milling contour (G100)
 Milling contour (G101, G102, G103)
 Conclusion of milling contour (G80)
Preferentially use ICP and the G840, G845 and G846
cycles to program the contour description in the geometry
section.
Parameters
ZS
Milling top edge
ZE
Milling floor
P
Maximum approach (default: total depth in one infeed)
U
Overlap factor—contour milling or pocket milling (default: 0)
R
I
K
F
E
H
 U=0: Contour milling
 U>0: Pocket milling—minimum overlap of milling paths =
U*milling diameter
Approach radius (radius of approaching/departing arc)—
(default: 0)
 R=0: Contour element is approached directly; infeed to
starting point above the milling plane—then vertical plunge
 R>0: Tool moves on approaching/departing arc that
connects tangentially to the contour element
 R<0 for inside corners: Tool moves on approaching/
departing arc that connects tangentially to the contour
element
 R<0 for outside corners: Length of linear approaching/
departing element; contour element is approached/departed
tangentially
Contour-parallel oversize
Oversize Z
Infeed rate
Reduced feed rate for circular elements (default: current feed
rate)
Cutting direction (default: 0): The cutting direction can be
changed with H and the direction of tool rotation.
 0: Up-cut milling
 1: Climb milling
HEIDENHAIN MANUALplus 620, CNC PILOT 640
351
4.26 Milling cycles
Parameters
Q
Cycle type (default: 0): Depending on U, the following applies:
 Contour milling (U=0)
 Q=0: Center of milling cutter on the contour
 Q=1, closed contour: Inside milling
 Q=1, open contour: Left in machining direction
 Q=2, closed contour: Outside milling
 Q=2, open contour: Right in machining direction
 Q=3, open contour: Milling location depends on "H" and
the direction of tool rotation—see help graphic
O
 Pocket milling (U>0)
 Q=0: From the inside toward the outside
 Q=1: From the outside toward the inside
Roughing/finishing
 0: Roughing. With each infeed, the complete surface is
machined.
 1: Finishing. The surface is machined with the last infeed. In
all previous infeeds, the cycle machines only the contour.
 Milling depth: The cycle calculates the depth from the
Milling top edge and the Milling floor—taking the
oversizes into account.
 Milling cutter radius compensation: Effective (except
for contour milling with Q=0).
 Approach and departure: For closed contours, the
point of the surface normal from the tool position to the
first contour element is the point of approach and
departure. If no surface normal intersects the tool
position, the starting point of the first element is the
point of approach and departure. For contour milling and
finishing (pocket milling), define with the Approach
radius whether the tool is to approach directly or in an
arc.
 G57/G58 oversizes are taken into account if the
Oversizes I, K are not programmed:
 G57: Oversize in X and Z direction
 G58: The oversize "shifts" the milling contour as
follows:
– With inside milling and closed contour: The contour
is contracted
– With outside milling and closed contour: The
contour is expanded
– With open contour and Q=1: Left in machining
direction
– With open contour and Q=2: Right in machining
direction
352
DIN Programming
4.26 Milling cycles
Contour and figure milling cycle, lateral surface
G794
G794 mills figures or (open or closed) "free" contours.
G794 is followed by:
 The figure to be milled with:
 Contour definition of the figure (G311 to G317)—See "Lateral
surface contours" on page 239.
 Conclusion of contour definition (G80)
 The free contour with:
 Starting point (G110)
 Contour definition (G111, G112, G113)
 Conclusion of contour definition (G80)
Preferentially use ICP and the G840, G845 and G846
cycles to program the contour description in the geometry
section.
Parameters
XS
Milling top edge (diameter value)
XE
Milling floor (diameter value)
P
Maximum approach (default: total depth in one infeed)
U
Overlap factor—contour milling or pocket milling (default: 0)
R
I
K
F
E
H
 U=0: Contour milling
 U>0: Pocket milling—minimum overlap of milling paths =
U*milling diameter
Approach radius (radius of approaching/departing arc)—
(default: 0)
 R=0: Contour element is approached directly; infeed to
starting point above the milling plane—then vertical plunge
 R>0: Tool moves on approaching/departing arc that
connects tangentially to the contour element
 R<0 for inside corners: Tool moves on approaching/
departing arc that connects tangentially to the contour
element
 R<0 for outside corners: Length of linear approaching/
departing element; contour element is approached/departed
tangentially
Oversize X
Contour-parallel oversize
Infeed rate
Reduced feed rate for circular elements (default: current feed
rate)
Cutting direction (default: 0): The cutting direction can be
changed with H and the direction of tool rotation.
 0: Up-cut milling
 1: Climb milling
HEIDENHAIN MANUALplus 620, CNC PILOT 640
Beispiel: G794
%314_G315.nc
[G314 / G315]
N1 T7 G197 S1200 G195 F0.2 M104
N2 M14
N3 G110 C0
N4 G0 X110 Z5
N5 G794 XS100 XE97 P2 U0.5 R0 K0.5 F0.15
N6 G314 Z-35 C0 R20
N7 G80
N8 M15
END
353
4.26 Milling cycles
Parameters
Q
Cycle type (default: 0): Depending on U, the following applies:
 Contour milling (U=0)
 Q=0: Center of milling cutter on the contour
 Q=1, closed contour: Inside milling
 Q=1, open contour: Left in machining direction
 Q=2, closed contour: Outside milling
 Q=2, open contour: Right in machining direction
 Q=3, open contour: Milling location depends on "H" and
the direction of tool rotation—see help graphic
O
 Pocket milling (U>0)
 Q=0: From the inside toward the outside
 Q=1: From the outside toward the inside
Roughing/finishing
 0: Roughing. With each infeed, the complete surface is
machined.
 1: Finishing. The surface is machined with the last infeed. In
all previous infeeds, the cycle machines only the contour.
 Milling depth: The cycle calculates the milling depth
from the Milling top edge and the Milling floor—
taking the oversizes into account.
 Milling cutter radius compensation: Effective (except
for contour milling with Q=0).
 Approach and departure: For closed contours, the
point of the surface normal from the tool position to the
first contour element is the point of approach and
departure. If no surface normal intersects the tool
position, the starting point of the first element is the
point of approach and departure. For contour milling and
finishing (pocket milling), define with the Approach
radius whether the tool is to approach directly or in an
arc.
 G57/G58 oversizes are taken into account if the
Oversizes I, K are not programmed:
 G57: Oversize in X and Z direction
 G58: The oversize "shifts" the milling contour as
follows:
– With inside milling and closed contour: The contour
is contracted
– With outside milling and closed contour: The
contour is expanded
– With open contour and Q=1: Left in machining
direction
– With open contour and Q=2: Right in machining
direction
354
DIN Programming
4.26 Milling cycles
Area milling, face G797
Depending on Q, G797 mills surfaces, a polygon, or the figure defined
in the command following G797.
Parameters
ID
Milling contour—name of the contour to be milled
NS Block number—beginning of contour section
X
ZS
ZE
B
V
R
A
Q
P
U
I
K
F
E
H
 Figures: Block number of the figure
 Free closed contour: First contour element (not starting
point)
Limit diameter
Milling top edge
Milling floor
Width across flats (omit for Q=0): B defines the remaining
material. For an even number of surfaces, you can program B
as an alternative to V.
 Q=1: B=residual depth
 Q>=2: B=width across flats
Edge length (omitted for Q=0)
Chamfer/rounding
Inclination angle (reference: see help graphic)—omitted for
Q=0
Number of surfaces (default: 0): Range: 0 <= Q <= 127
 Q=0: G797 is followed by a figure definition (G301.. G307,
G80) or a closed contour definition (G100, G101 to G103,
G80)
 Q=1: One surface
 Q=2: Two surfaces offset by 180°
 Q=3: Triangle
 Q=4: Rectangle, square
 Q>4: Polygon
Maximum approach (default: total depth in one infeed)
Overlap factor (default: 0.5): Minimum overlap of milling paths
= U*milling diameter
Contour-parallel oversize
Oversize Z
Infeed rate
Reduced feed rate for circular elements (default: current feed
rate)
Cutting direction (default: 0): The cutting direction can be
changed with H and the direction of tool rotation (see help
graphic)
 0: Up-cut milling
 1: Climb milling
HEIDENHAIN MANUALplus 620, CNC PILOT 640
355
4.26 Milling cycles
Beispiel: G797
Parameters
O
Roughing/finishing
J
 0: Roughing. With each infeed, the complete surface is
machined.
 1: Finishing. The surface is machined with the last infeed. In
all previous infeeds, the cycle machines only the contour.
Milling direction. For polygons without chamfers/rounding
arcs, J defines whether a unidirectional or bidirectional milling
operation is to be executed (see help graphic).
 0: Unidirectional
 1: Bidirectional
Programming notes:
The cycle calculates the milling depth from ZS and ZE, taking the
oversizes into account.
Surfaces and figures defined with G797 (Q>0) are symmetric with
respect to the center. A figure defined in the following command can
be outside the center.
G797 Q0 .. is followed by:
%797.nc
[G797]
N1 T9 G197 S1200 G195 F0.2 M104
N2 M14
N3 G110 C0
N4 G0 X100 Z2
N5 G797 X100 Z0 ZE-5 B50 R2 A0 Q4 P2 U0.5
N6 G100 Z2
N7 M15
END
Beispiel: G797/G304
%304_G305.nc
[G304]
N1 T7 G197 S1200 G195 F0.2 M104
 The figure to be milled with:
 Contour definition of the figure (G301 to G307)—See "Front and
rear face contours" on page 230.
 Conclusion of milling contour (G80)
N2 M14
 The free contour with:
 Starting point of milling contour (G100)
 Milling contour (G101, G102, G103)
 Conclusion of milling contour (G80)
N6 G304 XK20 YK5 R20
N3 G110 C0
N4 G0 X100 Z2
N5 G797 X100 ZS0 ZE-5 Q0 P2 F0.15
N7 G80
N4 G0 X100 Z2
N5 G797 X100 ZS0 ZE-5 Q0 P2 F0.15
N6 G305 XK20 YK5 R6 B30 K45 A20
N7 G80
N8 M15
END
356
DIN Programming
4.26 Milling cycles
Helical-slot milling G798
G798 mills a helical slot from the current tool position to the Final
point X, Z. The slot width equals the diameter of the milling cutter.
Parameters
X
Final point (diameter value)—(default: current X position)
Z
Final point of slot
C
Starting angle
F
Thread pitch:
P
K
U
I
E
D
 F positive: Right-hand thread
 F negative: Left-hand thread
Slop. length (run-in length)—ramp at the beginning of the slot
(default: 0)
End. length (run-out length)—ramp at the end of the slot
(default: 0)
Thread depth
Maximum approach (default: total depth in one infeed)
Reduction value for infeed reduction (default: 1)
No. of gears (threads per unit)
Infeeds:
 Infeed I is used for the first infeed movement.
 The Steuerung calculates all subsequent infeed movements as
follows:
Current infeed = I * (1 – (n–1) * E)
(n: nth infeed)
 The infeed movement is reduced down to >= 0.5 mm. Following
that, each infeed movement will amount to 0.5 mm.
You can mill a helical slot only from the outside.
Beispiel: G798
%798.nc
[G798]
N1 T9 G197 S1200 G195 F0.2 M104
N2 M14
N3 G110 C0
N4 G0 X80 Z15
N5 G798 X80 Z-120 C0 F20 K20 U5 I1
N6 G100 Z2
N7 M15
END
HEIDENHAIN MANUALplus 620, CNC PILOT 640
357
4.26 Milling cycles
Contour milling G840
G840—Fundamentals
G840 mills or deburrs open or closed contours (figures or "free
contours").
Plunge strategies: Depending on the cutter you are using, select one
of the following strategies:
 Vertical plunge: The cycle moves the tool to the starting point; the
tool plunges and mills the contour.
 Calculate positions, predrill, mill. The machining process is
performed in the following steps:
 Insert drill.
 Calculate hole positions with "G840 A1 ..".
 Predrill with "G71 NF .."
 Call cycle "G840 A0 ..". The cycle positions the tool above the hole;
the tool plunges and mills the contour.
 Predrilling, milling. The machining process is performed in the
following steps:
 Predrill with "G71 .."
 Position the cutter above the hole. Call cycle "G840 A0 ..". The
cycle plunges and mills the contour or contour section.
If the milling contour consists of multiple sections, G840 takes all the
sections of the contour into account for predrilling and milling. Call
"G840 A0 .." separately for each section when calculating the hole
positions without "G840 A1 ..".
Oversize: A G58 oversize "shifts" the contour to be milled in the
direction given in cycle type Q.
 With inside milling and closed contour: Shifted inward
 With outside milling and closed contour: Shifted outward
 Open contour: Shifts to the left or right depending on Q
 If Q=0, oversizes are not taken into account.
 G57 and negative G58 oversizes are not taken into
account.
358
DIN Programming
4.26 Milling cycles
G840—Calculating hole positions
"G840 A1 .." calculates the hole positions and stores them at the
reference specified in "NF." Program only the parameters given in the
following table.
See also:
 G840—Fundamentals: Page 358
 G840—Milling: Page 361
Parameters—Calculating hole positions
Q
Cycle type (= milling location)
 Open contour. If there is any overlapping, Q defines whether
the first section (as of starting point) or the entire contour is
to be machined.
 Q=0: Center of milling cutter on the contour (hole position
= starting point)
 Q=1: Machining at the left of the contour. If there is any
overlapping, only the first area of the contour is machined.
 Q=2: Machining at the right of the contour. If there is any
overlapping, only the first area of the contour is machined.
 Q=3: Not allowed
 Q=4: Machining at the left of the contour. If there is any
overlapping, the entire contour is machined.
 Q=5: Machining at the right of the contour. If there is any
overlapping, the entire contour is machined.
ID
NS
 Closed contours
 Q=0: Center of milling cutter on the contour (hole position
= starting point)
 Q=1: Inside milling
 Q=2: Outside milling
 Q=3 to 5: Not allowed
Milling contour—name of the contour to be milled
Contour start block number—beginning of contour section
NE
 Figures: Block number of the figure
 Free closed contour: First contour element (not starting
point)
 Open contour: First contour element (not starting point)
Contour end block number—end of contour section
 Figures, free closed contour: No input
 Open contour: last contour element
 Contour consists of one element:
 No input: Machining in contour direction
 NS=NE programmed: Machining against the contour
direction
HEIDENHAIN MANUALplus 620, CNC PILOT 640
359
4.26 Milling cycles
Parameters—Calculating hole positions
D
Starting element number for partial figures
The direction of contour definition for figures is
counterclockwise. The first contour element for figures:
V
A
NF
WB
 Circular slot: The larger arc
 Full circle: The upper semicircle
 Rectangles, polygons and linear slots: The orientation angle
points to the first contour element.
Ending element number for partial figures
Sequence for "Calculate hole positions": A=1
Position mark—reference at which the cycle stores the hole
positions [1 to 127].
Rework diameter—diameter of the milling cutter
Program D and V to machine parts of a figure.
 The cycle takes the diameter of the active tool into
account when calculating the hole positions. Therefore,
you need to insert the drill before calling "G840 A1 ..".
 Program oversizes for calculating the hole positions and
for milling.
G840 overwrites any hole positions that may still be stored
at the reference "NF."
360
DIN Programming
4.26 Milling cycles
G840—Milling
You can change the machining direction and the milling cutter radius
compensation (MCRC) with the cycle type Q, the cutting direction
H and the rotational direction of the tool (see table). Program only the
parameters given in the following table.
See also:
 G840—Fundamentals: Page 358
 G840—Calculating hole positions: Page 359
Parameters—Milling
Q
Cycle type (= milling location).
 Open contour. If there is any overlapping, Q defines whether
the first section (as of starting point) or the entire contour is
to be machined.
 Q=0: Center of milling cutter on the contour (without
MCRC)
 Q=1: Machining at the left of the contour. If there is any
overlapping, G840 machines only the first section of the
contour (starting point: 1st point of intersection).
 Q=2: Machining at the right of the contour. If there is any
overlapping, G840 machines only the first section of the
contour (starting point: 1st point of intersection).
 Q=3: The contour is machined to the left or right
depending on H and the direction of cutter rotation (see
table). If there is any overlapping, G840 machines only the
first section of the contour (starting point: 1st point of
intersection).
 Q=4: Machining at the left of the contour. If there is any
overlapping, G840 machines the entire contour.
 Q=5: Machining at the right of the contour. If there is any
overlapping, G840 machines the entire contour.
ID
NS
 Closed contours
 Q=0: Center of milling cutter on the contour (hole position
= starting point)
 Q=1: Inside milling
 Q=2: Outside milling
 Q=3 to 5: Not allowed
Milling contour—name of the contour to be milled
Block number—beginning of contour section
 Figures: Block number of the figure
 Free open or closed contour: First contour element (not
starting point)
HEIDENHAIN MANUALplus 620, CNC PILOT 640
361
4.26 Milling cycles
Parameters—Milling
NE
Block number—end of contour section
H
I
F
E
R
 Figures, free closed contour: No input
 Free open contour: Last contour element
 Contour consists of one element:
 No input: Machining in contour direction
 NS=NE programmed: Machining against the contour
direction
Cutting direction (default: 0)
 0: Up-cut milling
 1: Climb milling
(Maximum) infeed (default: milling in one infeed)
Infeed rate (depth infeed)—(default: active feed rate)
Reduced feed rate for circular elements (default: current feed
rate)
Radius of approaching/departing arc (default: 0)
RB
 R=0: Contour element is approached directly; infeed to
starting point above the milling plane, then vertical plunge.
 R>0: Tool moves on approaching/departing arc that
connects tangentially to the contour element.
 R<0 for inside corners: Tool moves on approaching/
departing arc that connects tangentially to the contour
element.
 R<0 for outside corners: Contour element is approached/
departed tangentially on a linear path
Milling depth (default: depth from the contour description)
Milling top edge—lateral surface (replaces the reference plane
from the contour definition)
Milling top edge—face (replaces the reference plane from the
contour definition)
Retraction plane (default: back to starting position)
D
V
 Front or rear face: Retraction position in Z direction
 Lateral surface: Retraction position in X direction (diameter)
Starting element number when partial figures are machined.
End element number when partial figures are machined.
P
XS
ZS
The direction of contour definition for figures is
counterclockwise. The first contour element for figures:
A
NF
362
 Circular slot: The larger arc
 Full circle: The upper semicircle
 Rectangles, polygons and linear slots: The orientation angle
points to the first contour element.
Sequence for "Milling, deburring": A=0 (default=0)
Position mark—reference from which the cycle reads the hole
positions [1 to 127].
DIN Programming
4.26 Milling cycles
Parameters—Milling
O
Plunging behavior (default: 0)
 O=0: Vertical plunging
 O=1: With predrilling
 If NF is programmed: The cycle positions the milling cutter
above the first hole position saved in NF, then plunges and
mills the first section. If applicable, the cycle positions the
tool to the next pre-drilled hole and mills the next section,
etc.
 If NF is not programmed: The tool plunges at the current
position and mills the section. If required, repeat this
operation for the next section, etc.
Approach and departure: For closed contours, the point of the
surface normal from the tool position to the first contour element is
the point of approach and departure. If no surface normal intersects
the tool position, the starting point of the first element is the point of
approach and departure. For figures, use D and V to select the
approach/departure element.
Cycle run for milling
1 Starting position (X, Z, C) is the position before the cycle begins.
2 Calculates the milling depth infeeds.
3 Approaches to safety clearance.
4
5
6
7
 If O=0: Infeed to the first milling depth.
 If O=1: Plunges to the first milling depth.
Mills the contour.
 For open contours and slots with slot width equal to the cutter
diameter: Advances to the next milling depth, or plunges to the
next milling depth and mills the contour in reverse direction.
 For closed contours and slots: Retracts by the safety clearance,
returns and advances to the next milling depth, or plunges to
the next milling depth.
Repeats steps 4 and 5 until the complete contour is milled.
Returns to retraction plane RB.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
363
4.26 Milling cycles
You can change the machining direction and the milling cutter
radius compensation (MCRC) with the cycle type Q, the cutting
direction H and the rotational direction of the tool (see following
table). Program only the parameters given in the following table.
Contour milling G840
Cycle
type
Cutting
direction
Direction
of tool
rotation
MCRC
Direction
of tool
rotation
MCRC
Contour
(Q=0)
–
Mx03
Up-cut
milling
(H=0)
Mx04
Left
Contour
–
Outside
Climb
milling
(H=1)
Mx03
Left
Contour
–
Outside
Climb
milling
(H=1)
Mx04
Right
Mx04
–
Contour
(Q=0)
–
Mx03
–
Up-cut
milling
(H=0)
Mx03
Right
Contour
–
Mx04
–
Inside
Up-cut
milling
(H=0)
Mx04
Left
Right
(Q=3)
Up-cut
milling
(H=0)
Mx03
Right
Inside
Climb
milling
(H=1)
Mx03
Left
Left
(Q=3)
Up-cut
milling
(H=0)
Mx04
Left
Inside
Climb
milling
(H=1)
Mx04
Right
Left
(Q=3)
Climb
milling
(H=1)
Mx03
Left
Outside
(Q=2)
Up-cut
milling
(H=0)
Mx03
Right
Right
(Q=3)
Climb
milling
(H=1)
Mx04
Right
Cycle
type
Cutting
direction
–
Outside
Mx03
–
–
Mx04
Contour
–
Inside
(Q=1)
364
Execution
Execution
DIN Programming
4.26 Milling cycles
G840—Deburring
G840 deburrs when you program chamfer width B. If there is any
overlapping of the contour, specify with cycle type Q whether the first
section (as of starting point) or the entire contour is to be machined.
Program only the parameters given in the following table.
Parameters—Deburring
Q
Cycle type (= milling location).
 Open contour. If there is any overlapping, Q defines whether
the first section (as of starting point) or the entire contour is
to be machined.
 Q=0: Center of milling cutter on the contour (without
MCRC)
 Q=1: Machining at the left of the contour. If there is any
overlapping, G840 machines only the first section of the
contour (starting point: 1st point of intersection).
 Q=2: Machining at the right of the contour. If there is any
overlapping, G840 machines only the first section of the
contour (starting point: 1st point of intersection).
 Q=3: The contour is machined to the left or right
depending on H and the direction of cutter rotation (see
table). If there is any overlapping, G840 machines only the
first section of the contour (starting point: 1st point of
intersection).
 Q=4: Machining at the left of the contour. If there is any
overlapping, G840 machines the entire contour.
 Q=5: Machining at the right of the contour. If there is any
overlapping, G840 machines the entire contour.
ID
NS
 Closed contours
 Q=0: Center of milling cutter on the contour (hole position
= starting point)
 Q=1: Inside milling
 Q=2: Outside milling
 Q=3 to 5: Not allowed
Milling contour—name of the contour to be milled
Block number—beginning of contour section
NE
 Figures: Block number of the figure
 Free open or closed contour: First contour element (not
starting point)
Block number—end of contour section
E
 Figures, free closed contour: No input
 Free open contour: Last contour element
 Contour consists of one element:
 No input: Machining in contour direction
 NS=NE programmed: Machining against the contour
direction
Reduced feed rate for circular elements (default: current feed
rate)
HEIDENHAIN MANUALplus 620, CNC PILOT 640
365
4.26 Milling cycles
Parameters—Deburring
R
Radius of approaching/departing arc (default: 0)
P
XS
ZS
RB
B
J
 R=0: Contour element is approached directly; infeed to
starting point above the milling plane, then vertical plunge.
 R>0: Tool moves on approaching/departing arc that
connects tangentially to the contour element.
 R<0 for inside corners: Tool moves on approaching/
departing arc that connects tangentially to the contour
element.
 R<0 for outside corners: Contour element is approached/
departed tangentially on a linear path
Milling depth (indicated as a negative value)
Milling top edge—lateral surface (replaces the reference plane
from the contour definition)
Milling top edge—face (replaces the reference plane from the
contour definition)
Retraction plane (default: back to starting position)
 Front or rear face: Retraction position in Z direction
 Lateral surface: Retraction position in X direction (diameter)
Chamfer width when deburring the edges
Preparation diameter. For open contours, the contour to be
deburred is calculated from the programmed contour and J.
Remember that:
D
V
 J programmed: The cycle deburrs both sides of the slot (see
1 in the illustration).
 J not programmed: The deburring tool is so wide that both
sides of the slot are deburred in one pass (see 2 in the
illustration).
Starting element number when partial figures are machined.
End element number when partial figures are machined.
The direction of contour definition for figures is
counterclockwise. The first contour element for figures:
A
366
 Circular slot: The larger arc
 Full circle: The upper semicircle
 Rectangles, polygons and linear slots: The orientation angle
points to the first contour element.
Sequence for "Milling, deburring": A=0 (default=0)
DIN Programming
4.26 Milling cycles
Approach and departure: For closed contours, the point of the
surface normal from the tool position to the first contour element is
the point of approach and departure. If no surface normal intersects
the tool position, the starting point of the first element is the point of
approach and departure. For figures, use D and V to select the
approach/departure element.
Cycle run for deburring
1 Starting position (X, Z, C) is the position before the cycle begins.
2 Moves to the safety clearance and infeed to the first milling
depth.
3  J not programmed: Mills the programmed contour.
 J programmed, open contour: Calculates and mills the "new"
contour.
4 Returns to retraction plane RB.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
367
4.26 Milling cycles
Pocket milling, roughing G845
G840—Fundamentals
G845 roughs closed contours. Choose one of the following plunge
strategies, depending on the milling cutter you are using:
 Plunge vertically
 Plunge at a pre-drilled position
 Plunge in a reciprocating or helical motion
When "plunging at a pre-drilled position," you have the following
alternatives:
 Calculate positions, drill, mill. The machining process is
performed in the following steps:
 Insert drill.
 Calculate hole positions with "G845 A1 ..."
 Predrill with "G71 NF .."
 Call cycle "G845 A0 ..." The cycle positions the tool above the hole;
the tool plunges and mills the pocket.
 Drill, mill. The machining process is performed in the following
steps:
 Drill a hole inside the pocket with "G71 ..."
 Position the milling cutter above the hole and call "G845 A0 ..." The
tool plunges and mills the section.
If the pocket consists of multiple sections, G845 takes all the sections
of the pocket into account for drilling and milling. Call "G845 A0 .."
separately for each section when calculating the hole positions
without "G845 A1 ..".
G845 takes the following oversizes into account:
 G57: Oversize in X and Z direction
 G58: Equidistant oversize in the milling plane
Program oversizes for calculating the hole positions and
for milling.
368
DIN Programming
4.26 Milling cycles
G845—Calculating hole positions
"G845 A1 .." calculates the hole positions and stores them at the
reference specified in "NF." The cycle takes the diameter of the active
tool into account when calculating the hole positions. Therefore, you
need to insert the drill before calling "G845 A1 ..". Program only the
parameters given in the following table.
See also:
 G845—Fundamentals: Page 368
 G845—Milling: Page 370
Parameters—Calculating hole positions
ID
Milling contour—name of the contour to be milled
NS Starting block no. of contour
B
XS
ZS
I
K
Q
A
NF
WB
 Figures: Block number of the figure
 Free closed contour: A contour element (not starting point)
Milling depth (default: depth from the contour description)
Milling top edge—lateral surface (replaces the reference plane
from the contour definition)
Milling top edge—face (replaces the reference plane from the
contour definition)
Oversize in X direction (radius)
Oversize in Z direction
Machining direction (default: 0)
 0: From the inside out (from the inside towards the outside)
 1: From the outside in (from the outside towards the inside)
Sequence for "Calculate hole positions": A=1
Position mark—reference at which the cycle stores the hole
positions [1 to 127].
Plunge length—diameter of the milling cutter
 G845 overwrites any hole positions that may still be
stored at the reference "NF."
 The parameter "WB" is used both for calculating the hole
positions and for milling. When calculating the hole
positions, "WB" describes the diameter of the milling
cutter.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
369
4.26 Milling cycles
G845—Milling
You can change the milling direction with the cutting direction H,
the machining direction Q and the direction of tool rotation (see
following table). Program only the parameters given in the following
table.
See also:
 G845—Fundamentals: Page 368
 G845—Calculating hole positions: Page 369
Parameters—Milling
ID
Milling contour—name of the contour to be milled
NS
Starting block no. of contour
B
P
XS
ZS
I
K
U
V
H
 Figures: Block number of the figure
 Free closed contour: A contour element (not starting point)
Milling depth (default: depth from the contour description)
(Maximum) infeed (default: milling in one infeed)
Milling top edge—lateral surface (replaces the reference plane
from the contour definition)
Milling top edge—face (replaces the reference plane from the
contour definition)
Oversize in X direction (radius)
Oversize in Z direction
(Minimum) overlap factor. Defines the overlap of milling paths
(default: 0.5).
Overlap = U*milling diameter
Overrun factor (no effect with C-axis machining)
Cutting direction (default: 0)
RB
 0: Up-cut milling
 1: Climb milling
Feed rate for infeed (default: active feed rate)
Reduced feed rate for circular elements (default: current feed
rate)
Retraction plane (default: back to starting position)
Q
 Front or rear face: Retraction position in Z direction
 Lateral surface: Retraction position in X direction (diameter)
Machining direction (default: 0)
F
E
 0: From the inside out (from the inside towards the outside)
 1: From the outside in (from the outside towards the inside)
370
DIN Programming
4.26 Milling cycles
Parameters—Milling
A
Sequence for "Milling": A=0 (default=0)
NF
Position mark—reference from which the cycle reads the hole
positions [1 to 127].
O
Plunging behavior (default: 0)
O=0 (vertical plunge): The cycle moves the tool to the starting
point; the tool plunges at the feed rate for infeed and mills the
pocket.
O=1 (plunge at pre-drilled position):
 If "NF" is programmed: The cycle positions the milling cutter
above the first pre-drilled hole; the tool plunges and mills the
first area. If applicable, the cycle positions the tool to the
next pre-drilled hole and mills the next area, etc.
 If "NF" is not programmed: The tool plunges at the current
position and mills the area. If applicable, position the tool to
the next pre-drilled hole and mill the next area, etc.
O=2, 3 (helical plunge): The tool plunges at the angle "W" and
mills full circles with the diameter "WB." As soon as it reaches
the milling depth "P," the cycle switches to face milling.
 O=2—manually: The cycle plunges at the current position
and machines the area that can be reached from this
position.
 O=3—automatically: The cycle calculates the plunging
position, plunges and machines this area. The plunging
motion ends at the starting point of the first milling path, if
possible. If the pocket consists of multiple areas, the cycle
successively machines all the areas.
O=4, 5 (reciprocating linear plunge): The tool plunges at the
angle "W" and mills a linear path of the length "WB." You can
define the orientation angle in "WE." The cycle then mills along
this path in the opposite direction. As soon as it reaches the
milling depth "P," the cycle switches to face milling.
 O=4—manually: The cycle plunges at the current position
and machines the area that can be reached from this
position.
 O=5—automatically: The cycle calculates the plunging
position, plunges and machines this area. The plunging
motion ends at the starting point of the first milling path, if
possible. If the pocket consists of multiple areas, the cycle
successively machines all the areas. The plunging position is
determined from the type of figure and from "Q" as follows:
HEIDENHAIN MANUALplus 620, CNC PILOT 640
371
4.26 Milling cycles
Parameters—Milling
 Q0 (from the inside toward the outside):
– Linear slot, rectangle, polygon: Reference point of the
figure
– Circle: Circle center
– Circular slot, "free" contour: Starting point of the
innermost milling path
 Q1 (from the outside toward the inside):
– Linear slot: Starting point of the slot
– Circular slot, circle: Not machined
– Rectangle, polygon: Starting point of the first linear
element
– "Free" contour: Starting point of the first linear element
(at least one linear element must exist)
O=6, 7 (reciprocating circular plunge): The tool plunges at
the plunging angle "W" and mills a circular arc of 90°. The cycle
then mills along this path in the opposite direction. As soon as
it reaches the milling depth "P," the cycle switches to face
milling. "WE" defines the arc center, "WB" the arc radius.
W
WE
 O=6—manually: The tool position corresponds to the center
of the circular arc. The tool moves to the arc starting point
and plunges.
 O=7—automatically (only permitted for circular slots and
circles): The cycle calculates the plunging position on the
basis of "Q":
 Q0 (from the inside toward the outside):
– Circular slot: The circular arc lies on the curvature radius
of the slot
– Circle: Not permitted
 Q1 (from the outside toward the inside): Circular slot,
circle: The circular arc lies on the outermost milling path
Plunging angle in infeed direction
Orientation angle of the milling path/circular arc. Reference
axis:
 Front or rear face: Positive XK axis
 Lateral surface: Positive Z axis
Default orientation angle, depending on "O":
WB
372
 O=4: WE=0°
 O=5 and
 Linear slot, rectangle, polygon: WE= orientation angle of
the figure
 Circular slot, circle: WE=0°
 "Free" contour and Q0 (from the inside toward the
outside): WE=0°
 "Free" contour and Q1 (from the outside toward the
inside): Orientation angle of the starting element
Plunge length/plunge diameter (default: 1.5 * milling diameter)
DIN Programming
4.26 Milling cycles
For the machining direction Q=1 (from the outside toward
the inside), please note:
 The contour must start with a linear element.
 If the starting element is < WB, WB is reduced to the
length of the starting element.
 The length of the starting element must not be less than
1.5 times the diameter of the milling cutter.
Cycle run
1 Starting position (X, Z, C) is the position before the cycle begins.
2 Calculates the number of cuts (infeeds to the milling planes,
infeeds in the milling depths) and the plunging positions and paths
for reciprocating or helical plunges.
3 Approaches to safety clearance and, depending on O, feeds to
the first milling depth or approaches helically or on a reciprocating
path.
4 Mills a plane.
5 Retracts by the safety clearance, returns and cuts to the next
milling depth.
6 Repeats steps 4 and 5 until the complete surface is milled.
7 Returns to retraction plane RB.
You can change the milling direction with the cutting direction H, the
machining direction Q and the direction of tool rotation (see following
table). Program only the parameters given in the following table.
Pocket milling, roughing G845
Cutting
direction
Machining
direction
Up-cut milling
(H=0)
From inside
(Q=0)
Up-cut milling
(H=0)
Direction
of tool
rotation
Direction
of tool
rotation
Cutting
direction
Machining
direction
Mx03
Climb milling
(H=1)
From inside
(Q=0)
Mx03
From inside
(Q=0)
Mx04
Climb milling
(H=1)
From inside
(Q=0)
Mx04
Up-cut milling
(H=0)
From outside
(Q=1)
Mx03
Climb milling
(H=1)
From outside
(Q=1)
Mx03
Up-cut milling
(H=0)
From outside
(Q=1)
Mx04
Climb milling
(H=1)
From outside
(Q=1)
Mx04
Execution
HEIDENHAIN MANUALplus 620, CNC PILOT 640
Execution
373
4.26 Milling cycles
Pocket milling, finishing G846
G846 finish-machines closed contours.
If the pocket consists of multiple sections, G846 takes all the sections
of the pocket into account.
You can change the milling direction with the cutting direction H,
the machining direction Q and the direction of tool rotation (see
following table).
Parameters—finishing
ID
Milling contour—name of the contour to be milled
NS
Starting block no. of contour
B
P
XS
ZS
R
U
V
H
F
E
RB
 Figures: Block number of the figure
 Free closed contour: A contour element (not starting point)
Milling depth (default: depth from the contour description)
(Maximum) infeed (default: milling in one infeed)
Milling top edge—lateral surface (replaces the reference plane
from the contour definition)
Milling top edge—face (replaces the reference plane from the
contour definition)
Radius of approaching/departing arc (default: 0)
 R=0: Contour element is approached directly. Feed to the
starting point above the milling plane, then vertical plunge.
 R>0: Tool moves on approaching/departing arc that
connects tangentially to the contour element.
(Minimum) overlap factor. Defines the overlap of milling paths
(default: 0.5).
Overlap = U*milling diameter
Overrun factor—no effect with C-axis machining
Cutting direction (default: 0)
 0: Up-cut milling
 1: Climb milling
Feed rate for infeed (default: active feed rate)
Reduced feed rate for circular elements (default: current feed
rate)
Retraction plane (default: back to starting position)
 Front or rear face: Retraction position in Z direction
 Lateral surface: Retraction position in X direction (diameter)
374
DIN Programming
4.26 Milling cycles
Parameters—finishing
Q
Machining direction (default: 0)
O
 0: From the inside out (from the inside towards the outside)
 1: From the outside in (from the outside towards the inside)
Plunging behavior (default: 0)
 O=0 (vertical plunge): The cycle moves the tool to the
starting point; the tool plunges and finishes the pocket.
 O=1 (approaching arc with depth feed): When machining the
upper milling planes, the tool advances to the milling plane
and then approaches on an arc. When machining the bottom
milling plane, the tool plunges to the milling depth while
moving on the approaching arc (three-dimensional
approaching arc). You can use this approach behavior only in
conjunction with an approaching arc "R" and when machining
from the outside toward the inside (Q=1).
Cycle run
1 Starting position (X, Z, C) is the position before the cycle begins.
2 Calculates the number of cutting passes (infeeds to the milling
planes, infeeds in the milling depths).
3 Moves to the safety clearance and feeds to the first milling depth.
4 Mills a plane.
5 Retracts by the safety clearance, returns and cuts to the next
milling depth.
6 Repeats steps 4 and 5 until the complete surface is milled.
7 Returns to retraction plane RB.
You can change the milling direction with the cutting direction H,
the machining direction Q and the direction of tool rotation (see
following table).
Pocket milling, finishing G846
Direction of tool
Cutting direction
rotation
Execution
Cutting direction
Direction of tool
rotation
Up-cut milling
(H=0)
Mx03
Climb milling (H=1) Mx03
Up-cut milling
(H=0)
Mx04
Climb milling (H=1) Mx04
HEIDENHAIN MANUALplus 620, CNC PILOT 640
Execution
375
4.27 Engraving cycles
4.27 Engraving cycles
Character set
The Steuerung can realize the characters listed in the following table.
The text to be engraved is entered as a character string. Diacritics and
special characters that you cannot enter in the editor can be defined,
character by character, in NF. If text is defined in "ID" and a character
is defined in "NF," the text is engraved before the character.
NF
Character NF
Character
Numerals,
diacritics
NF
Character
97
a
65
A
48
0
32
98
b
66
B
49
1
37
%
Per cent sign
99
c
67
C
50
2
40
(
Opening parenthesis
100
d
68
D
51
3
41
)
Closing parenthesis
101
e
69
E
52
4
43
+
Plus character
102
f
70
F
53
5
44
,
Comma
103
g
71
G
54
6
45
–
Minus sign
104
h
72
H
55
7
46
.
Point
105
i
73
I
56
8
47
/
Forward slash
106
j
74
J
57
9
58
:
Colon
107
k
75
K
60
<
Less than character
108
l
76
L
196
Ä
61
=
Equal sign
109
m
77
M
214
Ö
62
>
Greater than character
110
n
78
N
220
Ü
64
@
at
111
o
79
O
223
ß
91
[
Opening brackets
112
p
80
P
228
ä
93
]
Closing brackets
113
q
81
Q
246
ö
95
_
Underscore
114
r
82
R
252
ü
8364
115
s
83
S
181
µ
Micro
116
t
84
T
186
°
Degrees
117
u
85
U
215
*
Multiplication sign
118
v
86
V
33
!
Exclamation point
Small letters
376
Capital letters
Special
characters
NF
Character
Meaning
Space
Euro sign
DIN Programming
Capital letters
Numerals,
diacritics
NF
Character
Special
characters
NF
Character
Meaning
NF
Character NF
Character
119
w
87
W
38
&
Ampersand and
120
x
88
X
63
?
Question mark
121
y
89
Y
174
®
Trademark
122
z
90
Z
216
Ø
Diameter sign
HEIDENHAIN MANUALplus 620, CNC PILOT 640
4.27 Engraving cycles
Small letters
377
4.27 Engraving cycles
Engraving on front face G801
G801 engraves character strings in linear or polar layout on the front
face. For character set and more information, see page 376
The cycles start engraving from the starting position or from the
current position, if no starting position is defined.
Example: If a character string is engraved with several calls, define the
starting position in the first call. All other calls are programmed without
a starting position.
Parameters
X, C
Polar starting point
XK, YK
Cartesian starting point
Z
End point. Z position, infeed depth during milling.
RB
Retraction plane. Z position retracted to for positioning.
ID
Text to be engraved
NF
Character number (character to be engraved)
W
Inclination angle. Example: 0° = Vertical characters: the
characters are aligned in sequence in positive X direction
H
Font height
E
Distance factor (for calculation see figure)
V
Execution
D
F
378
 0: Linear
 1: Arched above
 2: Arched below
Reference diameter
Plunging feed rate factor (plunging feed rate = current
feed rate * F)
DIN Programming
4.27 Engraving cycles
Engraving on lateral surface G802
G802 engraves character strings aligned linearly on the lateral surface.
For character set and more information, see page 376
The cycles start engraving from the starting position or from the
current position, if no starting position is defined.
Example: If a character string is engraved with several calls, define the
starting position in the first call. All other calls are programmed without
a starting position.
Parameters
Z
Starting point
C
Starting angle
CY
Starting point
X
End point (diameter). X position, infeed depth during milling.
RB Retraction plane. X position retracted to for positioning.
ID
Text to be engraved
NF
Character number. ASCII code of the character to be engraved
W
Inclination angle
H
Font height
E
Distance factor (for calculation see figure)
D
Reference diameter
F
Plunging feed rate factor (plunging feed rate = current feed
rate * F)
HEIDENHAIN MANUALplus 620, CNC PILOT 640
379
4.28 Contour follow-up
4.28 Contour follow-up
Automatic contour follow-up is not possible with program branches or
repetitions. In these cases you control the contour follow up with the
following commands.
Saving/loading contour follow-up G702
G702 saves the current contour or loads a saved contour.
Parameters
ID
Workpiece blank contour—name of the auxiliary workpiece
blank
Q
Save/load contour
H
V
 0: Saves the current contour. The contour follow-up is not
affected.
 1: Loads the specified contour. The contour follow-up is
continued with the loaded contour.
 2: The following cycle uses the "internal workpiece blank."
Memory number (0 .. 9)
The following information is saved:
 0: Everything (variable contents and workpiece blank
contours)
 1: Variable contents
 2: Workpiece blank contours
G702 Q=2 switches off the global contour follow-up for the following
cycle. Once the cycle has been executed, the global contour follow-up
is effective again.
The affected cycle uses the "internal workpiece blank." The cycle
determines the internal workpiece blank from the contour and the tool
position.
G702 Q2 must be programmed before the cycle.
Contour follow-up on/off G703
G703 is used to deactivate/reactivate the contour follow-up.
Parameters
Q
Contour follow-up on/off
 0: Off
 1: On
380
DIN Programming
4.29 Other G codes
4.29 Other G codes
Chucking equipment in simulation G65
G65 displays the selected chucking equipment in the simulation
graphics.
Parameters
H
No. of clamping (no. of chuck) (always program H=0)
D
No. of spindle—No input:
X
Diameter of workpiece blank
Z
Start point—No input
Q
Chuck form
B
P
V
 4: Externally clamped
 5: Internally clamped
Clamping length (B+P = length of blank)
Free length
Delete chucking equipment
Workpiece blank contour G67 (for graphics)
G67 displays an auxiliary workpiece blank in the simulation graphics.
Parameters
ID
ID of auxiliary workpiece blank
NS Block number of contour
Period of dwell G4
With G4, the Steuerung interrupts the program run for the time F or
until the revolutions on the recess floor D have been completed before
executing the next program block. If G4 is programmed together with
a path of traverse in the same block, the dwell time or the number of
revolutions on the recess floor only become effective after the path of
traverse has been executed.
Parameters
F
Dwell time [sec] (0 < F <= 999)
D
Revolutions on recessing floor
Precision stop G7
G7 switches precision stop on. It is a modal function. With a precision
stop, the Steuerung does not run the following block until the last
point has been reached in the tolerance window for position. The
tolerance window is a configuration parameter ("ParameterSets
PX(PZ)/CfgControllerTol/posTolerance").
Precision stop affects single paths and cycles. The NC block
containing G7 is also executed with a precision stop.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
381
4.29 Other G codes
Precision stop off G8
G8 switches precision stop off. The block containing G8 is executed
without a precision stop.
Precision stop G9
G9 activates a precision stop for the NC block in which it is
programmed. With a precision stop, the Steuerung does not run the
following block until the last point has been reached in the tolerance
window for position. The tolerance window is a configuration
parameter ("ParameterSets PX / PZ > CfgControllerTol >
posTolerance").
Switch off protection zone G60
G60 is used to cancel protection zone monitoring. G60 is programmed
before the traversing command to be monitored or not monitored.
Parameters
Q
Activate/Deactivate
 0: Activate protection zone (modal)
 1: Deactivate protection zone (modal)
Application example: With G60, you can temporarily deactivate a
programmed monitoring of the protection zone in order to machine a
centric through hole.
Beispiel: G60
...
N1 T4 G97 S1000 G95 F0.3 M3
N2 G0 X0 Z5
N3 G60 Q1 [Deactivate the protection zone]
N4 G71 Z-60 K65
N5 G60 Q0 [Activate the protection zone]
...
Actual values in variables G901
G901 transfers the actual values of all the axes of a slide into the
variables for the interpolation information.
See G904 Page 383.
Zero-point shift in variables G902
G902 transfers the zero-point shifts into the variables for the
interpolation information.
See G904 Page 383.
Lag error in variables G903
G903 transfers the current following error (distance by which the
actual values lags the nominal value) into the variables for the
interpolation information.
See G904 Page 383.
382
DIN Programming
4.29 Other G codes
Read interpolation information G904
G904 transfers all the current interpolation information on the current
slide to the variable memory.
Interpolation information
#a0(Z,1)
Zero-point shift of the Z axis of slide $1
#a1(Z,1)
Actual position of the Z axis of slide $1
#a2(Z,1)
Nominal position of the Z axis of slide $1
#a3(Z,1)
Lag error of the Z axis of slide $1
#a4(Z,1)
Distance to go in the Z axis of slide $1
#a5(Z,1)
Logical axis number of the Z axis of slide $1
#a5(0,1)
Logical axis number of the main spindle
#a6(0,1)
Rotational direction of main spindle $1
#a9(Z,1)
Trigger position of the touch probe
#a10(Z,1)
IPO axis value
Interpolation information syntax
Syntax:
#an(axis,channel)
 n = number of the information
 axis = name of the axis
 channel = slide number
Feed rate override 100 % G908
G908 sets the feed override for traverse paths (G0, G1, G2, G3, G12,
G13) block by block to 100 %.
Program G908 and the traverse path in the same NC block.
Interpreter stop G909
The Steuerung pre-interprets the NC blocks. If variables are assigned
shortly before the evaluation, "old values" would be processed. G909
stops the pre-interpretation. The NC blocks are processed up to G909.
Only after G909, are the subsequent NC blocks processed.
Apart from G909, the NC block should only contain synchronous
functions. (Some G codes generate an interpreter stop.)
Spindle override 100 % G919
G919 is used to deactivate/activate the spindle speed override.
Parameters
Q
Spindle number (default: 0)
H
Type of limit (default: 0)
 0: Activate spindle speed override
 1: Spindle override at 100 %—modal
 2: Spindle override at 100 %—for the current NC block
HEIDENHAIN MANUALplus 620, CNC PILOT 640
383
4.29 Other G codes
Deactivate zero-point shifts G920
G920 deactivates the workpiece zero point and zero-point shifts.
Traverse paths and position values are referenced to the distance
tool tip—machine zero point.
Deactivate zero-point shifts, tool lengths G921
G921 deactivates the workpiece zero point, zero-point shifts and tool
dimensions. Traverse paths and position values are referenced to the
slide reference point—machine zero point.
End position of tool G922
With G922 you can position the active tool to a defined angle.
Parameters
C
Angular position for tool orientation
Fluctuating spindle speed G924
To reduce resonant vibrations you can use G924 to program a
changing spindle speed. In G924 you define the time interval and the
range for the speed change. The G924 function is automatically reset
at the end of the program. You can also deactivate the function
through another call with the setting H=0 (off).
Parameters
Q
Spindle number (machine-dependent)
K
Repetition rate: Time interval in hertz (repetitions per
second)
I
Change of spindle speed
H
Switch on/off the G924 function
 0: Off
 1: On
384
DIN Programming
4.29 Other G codes
Convert lengths G927
Function G927 is used to convert the tool lengths at the current tool
insert angle to the initial position of the tool (reference position in B
axis = 0).
The results can be interrogated in the variables #n927( X), #n927( Z),
and #n927( Y).
Parameters
H
Method of conversion:
 0: Convert tool length to reference position (take I + K of
the tool into account)
 1: Convert tool length to reference position (do not take I
+ K of the tool into account)
 2: Convert tool length from the reference position to the
current work position (take I + K of the tool into account)
 3: Convert tool length from the reference position to the
current work position (do not take I + K of the tool into
account)
X, Y, Z Axis values (X value = radius). If nothing is entered, the value
0 is used.
Calculate variables automatically G940
Use G940 to convert metric values to inch values. When you create a
new program you can select between metric units and inches.
Internally the control always calculates with metric values. If you read
out variables in an "inch" program, the variables are always output as
metric values. Use G940 to convert the variables to INCH values.
Parameters
H
Switch on/off the G940 function
 0: Unit conversion active
 1: Values remain metric
In inch programs, a conversion is required for variables that refer to a
metric unit of measurement:
Machine dimensions
#m1(n)
Machine dimensions of an axis, e.g. #m1(X) for
machine dimensions of the X axis
Reading tool data
#wn(NL)
Usable length (inside turning and drilling tools)
#wn(RS)
Cutting edge radius
#wn(ZD)
Stud diameter
#wn(DF)
Cutter diameter
#wn(SD)
Shank diameter
HEIDENHAIN MANUALplus 620, CNC PILOT 640
385
4.29 Other G codes
Reading tool data
#wn(SB)
Cutting width
#wn(AL)
Length of first cut
#wn(FB)
Cutter width
#wn(ZL)
Tool setting dimension in Z
#wn(XL)
Tool setting dimension in X
#wn(YL)
Tool setting dimension in Y
#wn(I)
Position of tool tip center in X
#wn(K)
Position of tool tip center in Z
#wn(ZE)
Distance between tool tip and slide zero point Z
#wn(XE)
Distance between tool tip and slide zero point X
#wn(YE)
Distance between tool tip and slide zero point Y
Reading the current NC information
#n0(Z)
Last programmed position Z
#n120(X)
Reference diameter X for calculating CY
#n57(X)
Oversize in X
#n57(Z)
Oversize in Z
#n58(P)
Equidistant oversize
#n150(X)
Cutting width shifted in X by G150
#n95(F)
Last programmed feed rate
#n47(P)
Current safety clearance
#n147(I)
Current safety clearance in working plane
#n147(K)
Current safety clearance in infeed direction
Internal information for defining constants
__n0_x
768 Last programmed position X
__n0_y
769 Last programmed position Y
__n0_z
770 Last programmed position Z
__n120_x
787 Reference diameter X for calculating CY
__n57_x
791 Oversize in X
__n57_z
792 Oversize in Z
386
DIN Programming
4.29 Other G codes
Internal information for defining constants
__n58_p
793 Equidistant oversize
__n150_x
794 Cutting width shifted in X by G150/G151
__n150_z
795 Cutting width shifted in Z by G150/G151
__n95_f
800 Last programmed feed rate
Reading interpolation information G904
#a0(Z,1)
Zero-point shift of the Z axis of slide $1
#a1(Z,1)
Actual position of the Z axis of slide $1
#a2(Z,1)
Nominal position of the Z axis of slide $1
#a3(Z,1)
Lag error of the Z axis of slide $1
#a4(Z,1)
Distance to go in the Z axis of slide $1
Misalignment compensation G976
With the G976 function (misalignment compensation) you can run the
following operations on tapering contours (e.g. to counter a
mechanical offset). The G976 function is automatically reset at the end
of the program. You can also deactivate the function through another
call with the setting H=0 (off).
Parameters
Z
Starting point
K
Length
I
Incremental distance
J
Incremental distance
H
Switch on/off the G976 function
 0: Off
 1: On
Activate zero-point shifts G980
G980 activates the workpiece zero point and all zero-point shifts.
Traverse paths and position values are referenced to the distance of
the tool tip to the workpiece zero point, while taking the zero point
shifts into consideration.
Activate zero-point shifts, tool lengths G981
G981 activates the workpiece zero point, all zero-point shifts and the
tool dimensions. Traverse paths and position values are referenced to
the distance of the tool tip to the workpiece zero point, while taking
the zero point shifts into consideration.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
387
4.29 Other G codes
Monitoring zone G995
G995 defines the monitoring zone and the axes to be monitored. The
monitoring zone corresponds to the program section that is to be
monitored by the control.
To begin the monitoring zone, program G995 with the following
parameters. To end the monitoring zone, program G995 without
parameters.
Parameters
H
No. of the zone (range: 1 to 99)
ID
Code for axes
 X: X axis
 Y: Y axis
 Z: Z axis
 0: Spindle 1 (main spindle, C axis)
 1: Spindle 2
 2: Spindle 3
Beispiel: G995
...
N1 T4
N2 G995 H1 ID"X0" [Beginning of monitoring
zone; monitoring of X axis and main spindle]
. . . [Machining]
G995 [End of monitoring zone]
...
The monitoring zones must be unambiguously defined in
the program. Use the H parameter to assign a unique
number to each monitoring zone.
If you would like to monitor more than one drive within a
monitoring zone, enter the respective combination of
individual parameters in the ID parameter. Please keep in
mind, however, that the control can monitor a maximum
of four drives per monitoring zone. To simultaneously
monitor the Z axis and the main spindle, enter Z0 in the ID
parameter.
In addition to defining the monitoring zone with G995, you
need to activate the load monitoring function (see „Load
monitoring G996” on page 389).
388
DIN Programming
G996 defines the type of load monitoring or deactivates the load
monitoring temporarily.
Parameters
Q
Lib. switch (type of activation): Monitoring (default: 0)
Q
 0: Off
 1: G0 Off (do not monitor rapid traverse)
 2: G0 On (monitor rapid traverse)
Monitoring: Type of load monitoring (default: 0)
 0: Utilization + Total utilization
 1: Utilization only
 2: Total utilization only
Beispiel: G996
...
N1 G996 Q1 H1 [Activate load monitoring; do
not monitor rapid traverse]
N2 T4
N3 G995 H1 ID"X0"
. . . [Machining]
N9 G995
...
In addition to defining the type of load monitoring with
G996, you need to specify the monitoring zone with G995
(see „Monitoring zone G995” on page 388).
Before using the load monitoring feature, you also need to
define limit values and perform reference machining (see
User's Manual).
Activate direct program-run continuation G999
With the G999 function, when running a program in Single Block
mode, the following NC blocks are run with a single NC start to the
end of the program. G999 is then deactivated by again calling the
function with the setting Q=0 (off).
Converting and mirroring G30
The G30 function converts G codes, M functions and spindle
numbers. G30 mirrors traverse paths and tool dimensions and shifts
the machine zero point about the "zero point offset" of the axis
(machine parameter: Trans_Z1).
Parameters
H
Table number of the conversion table (possible only if the
machine tool builder has configured a conversion table).
Q
Spindle number
Application: For full-surface machining, you describe the complete
contour, machine the front face, rechuck the workpiece through an
expert program and then machine the rear face. To enable you to
HEIDENHAIN MANUALplus 620, CNC PILOT 640
389
4.29 Other G codes
Load monitoring G996
4.29 Other G codes
program rear-face machining in the same way as front-face machining
(Z-axis orientation, arc rotational direction, etc.), the expert program
includes commands for converting and mirroring.
Danger of collision!
 In the transition from AUTOMATIC to MANUAL
OPERATION, conversions and mirror images are
retained
 Switch off the conversion/mirroring if you activate the
front-face machining after rear-face machining (for
example during program section repeats with M99)
 After a new program selection, the conversion/mirroring
is switched off (example: transition from MANUAL to
AUTOMATIC mode)
390
DIN Programming
4.29 Other G codes
Transformations of contours G99
With the G99 function you can mirror contours, shift them and bring
the workpiece to the desired machining position.
Parameters
Q
Function is not yet supported.
D
Spindle number
X
Shift in X (diameter value)
Z
Shift in Z
V
Mirroring the Z axis of the coordinate system
 Q=0: Do not mirror
 Q=1: Mirror
H
Transformation type
 H=0: Contour shift, not mirroring
 H=1: Contour shift, mirroring and reversing the direction
of the contour description
K
Length of workpiece shift: shift coordinate system in Z
direction
O
Hide elements during transformation
 O=0: All contours are transformed
 O=1: Auxiliary contours are not transformed
 O=2: Face contours are not transformed
 O=4: Lateral contours are not transformed
You can also add input values in order to combine various
settings (e.g. O=3 Do not transform auxiliary contours or
face contours)
 Program G99 again if the workpiece is transferred to
another spindle and/or moves its position in the working
space.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
391
4.29 Other G codes
Spindle synchronization G720
Machine and control must be specially prepared by the
machine tool builder for use of this cycle. Refer to your
machine manual.
G720 controls the workpiece transfer from the master to the slave
spindle and synchronizes functions such as polygonal turning jobs.
The function stays active until you deactivate G720 with the setting
H0.
If you would like to synchronize more than two spindles you can
program G720 several times in succession.
Parameters
S
Number of the master spindle
H
Number of the slave spindle—no input or H=0: Switches off
the spindle synchronization
C
Offset angle [°]
Q
Master spindle speed factor
Range: –100 <= Q <= 100
F
Slave spindle speed factor
Range: –100 <= F <= 100
Y
Type of cycle
Your machine manual provides more detailed information
about machine-dependent functions.
Program the speed of the master spindle with Gx97 S.. and define the
speed ratio between the master spindle and the slave spindle with Q,
F. If you enter a negative value for Q or F, the direction of rotation of
the slave spindle will be reversed.
Remember that: Q * master speed = F * slave speed
Example: G720
...
N.. G397 S1500 M3
Spindle speed and direction of rotation of master
spindle
N.. G720 C180 S0 H1 Q2 F-1
Synchronization of master spindle and slave
spindle. The slave spindle precedes the master
spindle by 180°. Slave spindle: direction of rotation
M4; spindle speed 750
N.. G1 X.. Z..
...
392
DIN Programming
4.29 Other G codes
C-angle offset G905
G905 measures the angular offset of workpiece transfer with rotating
spindle. The sum of angle C and the angle offset goes into effect as
the zero point shift of C axis. If you request the zero point shift of the
current C-axis in the variable #a0 ( C,1) the sum of the programmed
zero point shift and the measured offset angle is transferred.
The zero offset is effective internally as a direct zero point shift for the
respective C axis. The contents of the variables are retained even if the
control has been switched off.
You can also examine and reset the respectively active zero point shift
of the C axis in the "Setup" menu in the "Set C-axis value" function.
Parameters
Q
Number of the C axis
C
Angle of additional zero point shift for offset gripping (–360°
<= C <= 360°)—(default: 0°)
Danger of collision!
 For narrow workpieces the jaws have to grip at an
offset.
 The zero point shift of the C axis remains in effect:
 After switch from Automatic to Manual mode
 After switch-off
HEIDENHAIN MANUALplus 620, CNC PILOT 640
393
4.29 Other G codes
Traversing to a fixed stop G916
The machine tool builder determines the scope of function
and behavior of G916. The machine manual provides
further information.
G916 activates the monitoring function for the traversing path and
moves to a fixed stop (example: transferring a premachined workpiece
to a second traveling spindle if you do not know the exact position of
the workpiece).
The control stops the slide and saves the stop position. G916
generates an interpreter stop.
Parameters
H
Clamping force in daNewtons (1 daNewton = 10 newtons)
D
Axis number (X=1, Y=2, Z=3, U=4, V=5, W=6, A=7, B=8,
C=9)
K
Incremental distance
R
Return path of traverse
V
Type of departure
 V=0: Stay at fixed stop
 V=1: Return to start position
 V=2: Retract by return path R
O
Error evaluation
 O=0: Error evaluation in expert program
 O=1: The control issues an error message
Lag error monitoring is not activated until the acceleration
phase has been completed.
The feed rate override is not effective during cycle
execution.
394
DIN Programming
4.29 Other G codes
Traversing to a fixed stop
When traversing to a fixed stop, the control moves
 up to the fixed stop and stops as soon as the following error has
been reached. The remaining path of traverse is deleted
 back to starting position
 back by the return traverse path
Programming "traverse to a fixed stop":


Position the slide at a sufficient distance before the fixed stop.
Use a moderate feed rate (< 1000 mm/min)
Example of traversing to a fixed stop:
...
N.. G0 Z20
Pre-position slide 2
N.. G916 H100 D6 K-20 V0 O1
Activate monitoring, traverse to a fixed stop
...
HEIDENHAIN MANUALplus 620, CNC PILOT 640
395
4.29 Other G codes
Controlled parting using lag error monitoring
G917
The machine tool builder determines the scope of function
and behavior of G917. The machine manual provides
further information.
G917 "monitors" the path of traverse. The controlled parting function
(cut-off control) prevents collisions caused by incomplete parting
processes.
The control stops the slide when the tensile force is too high and
generates an "interpreter stop."
Parameters
H
Tensile force
D
Axis number (X=1, Y=2, Z=3, U=4, V=5, W=6, A=7, B=8,
C=9)
K
Incremental distance
O
Error evaluation
 O=0: Error evaluation in expert program
 O=1: The control issues an error message
During parting control, the parted workpiece moves in the positive Z
direction. If a following error occurs, the workpiece is considered
unparted.
The result is saved in the variable #i99:
 0: Workpiece was not correctly cut off (following error detected)
 1: Workpiece was correctly cut off (no following error detected)
Lag error monitoring is not activated until the acceleration
phase has been completed.
The feed rate override is not effective during cycle
execution.
396
DIN Programming
4.29 Other G codes
Force reduction G925
The machine tool builder determines the scope of function
and behavior of G925. The machine manual provides
further information.
G925 activates/deactivates the force reduction. When the monitoring
is activated, the maximum contact force for one axis is defined. Force
reduction can be activated for only one axis per NC channel.
The G925 function limits the contact force for subsequent movements
of the defined axis. G925 does not execute any traverse.
Parameters
H
Contact force [dN]—The contact force is limited to the
given value
Q
Axis number (X=1, Y=2, Z=3, U=4, V=5, W=6, A=7, B=8,
C=9)
Spindle number, e.g. spindle 0 = number 10 (0=10, 1=11,
2=12, 3=13, 4=14, 5=15)
S
Sleeve monitoring
 0: Deactivate (the contact force is not monitored)
 1: Activate (the contact force is monitored)
Lag error monitoring is not activated until the acceleration
phase has been completed.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
397
4.29 Other G codes
Sleeve monitoring G930
The machine tool builder determines the scope of function
and behavior of G930. The machine manual provides
further information.
G930 activates/deactivates the sleeve monitoring. When the
monitoring is activated, the maximum contact force for one axis is
defined. Sleeve monitoring can be activated for only one axis per NC
channel.
G930 moves the defined axis by the programmed distance D until the
defined contact force H has been reached.
Parameters
H
Contact force [dN]—The contact force is limited to the
given value
Q
Axis number (X=1, Y=2, Z=3, U=4, V=5, W=6, A=7, B=8,
C=9)
D
Incremental distance
Application example: G930 is applied to use the opposing spindle as
a mechatronic tailstock. In this case the opposing spindle is equipped
with a dead center and the contact force is limited with G930. A
prerequisite for this application is a PLC program from the machine
tool builder that enables the user to operate the mechatronic tailstock
in the Manual and Automatic operating mode.
Lag error monitoring is not activated until the acceleration
phase has been completed.
Tailstock function
With the tailstock function, the control moves up to the workpiece and
stops as soon as the contact force has been reached. The remaining
path of traverse is deleted.
Example of tailstock function
...
N.. G0 Z20
Pre-position slide 2
N.. G930 H250 D6 K-20
Activate the tailstock function—contact force
250 daN
...
398
DIN Programming
4.29 Other G codes
Eccentric turning G725
G725 is used to machine turning contours outside the original turning
center.
The turning contours are programmed using separate turning cycles.
Machine and control must be specially prepared by the
machine tool builder for use of this cycle. Refer to your
machine manual.
Prerequisites:
 Software option Y-Axis Machining
 Software option Synchronizing Functions
Parameters
H
Activate coupling
 H=0: Deactivate coupling
 H=1: Activate coupling
Q
Reference spindle: Number of the spindle that is coupled
with the X and Y axes (machine-dependent)
R
Center offset: Distance between the eccentric center and
the original turning center (radius value)
C
Position C: C-axis angle of the center offset
F
Maximum rapid traverse: Permissible rapid traverse for the
X and Y axes while coupling is active
V
Direction reversal in Y (machine-dependent)
 V=0: The control uses the configured axis direction for Yaxis movements
 V=1: The control reverses the configured axis direction
for Y-axis movements
Please note while programming:
 Program a workpiece blank increased by the center
offset in the radius if you are using turning cycles that
are referenced to the workpiece-blank definition.
 Program a starting point increased by the center offset
in the radius if you are using turning cycles that are not
referenced to the workpiece-blank definition.
 Reduce the spindle speed if you increase the center
offset.
 Reduce the maximum rapid traverse F if you increase
the center offset.
 Use identical values for the parameter Q when activating
and deactivating the coupling.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
399
4.29 Other G codes
Programming sequence:




Position the cursor in the MACHINING program section
Program G725 with H=1 (activate coupling)
Program turning cycles
Program G725 with H=0 (deactivate coupling)
Please note when executing the program:
 In the event of a program cancelation, the control
automatically deactivates the coupling.
400
DIN Programming
4.29 Other G codes
Transition to eccentric G726
G726 is used to machine turning contours outside the original turning
center. In addition, G726 offers the possibility to continuously change
the position of the turning center along a straight line or a curve.
The turning contours are programmed using separate turning cycles.
Machine and control must be specially prepared by the
machine tool builder for use of this cycle. Refer to your
machine manual.
Prerequisites:
 Software option Y-Axis Machining
 Software option Synchronizing Functions
Parameters
H
Activate coupling
 H=0: Deactivate coupling
 H=1: Activate coupling
Q
Reference spindle: Number of the spindle that is coupled
with the X and Y axes (machine-dependent)
R
Center offset at Z start: Distance between the eccentric
center and the original turning center (radius value)
C
C position at Z start: C-axis angle of the center offset
F
Maximum rapid traverse: Permissible rapid traverse for the
X and Y axes while coupling is active
V
Direction reversal in Y (machine-dependent)
 V=0: The control uses the configured axis direction for Yaxis movements
 V=1: The control reverses the configured axis direction
for Y-axis movements
Z
Z start: Reference value for the parameters R and C, as well
as coordinate for tool pre-positioning
K
Z end: Reference value for the parameters W and U
W
Delta C [Z start – Z end]: Difference in C-axis angle between
Z start and Z end
U
Center offset at Z end: Distance between the eccentric
center and the original turning center (radius value)
HEIDENHAIN MANUALplus 620, CNC PILOT 640
401
4.29 Other G codes
Please note while programming:
 Program a workpiece blank increased by the center
offset in the radius if you are using turning cycles that
are referenced to the workpiece-blank definition.
 Program a starting point increased by the center offset
in the radius if you are using turning cycles that are not
referenced to the workpiece-blank definition.
 Reduce the spindle speed if you increase the center
offset.
 Reduce the maximum rapid traverse F if you increase
the center offset.
 Use identical values for the parameter Q when activating
and deactivating the coupling.
Programming sequence:




Position the cursor in the MACHINING program section
Program G726 with H=1 (activate coupling)
Program turning cycles
Program G726 with H=0 (deactivate coupling)
Please note when executing the program:
 When the coupling is activated, the control positions the
tool in the Z axis to the value of the parameter Z.
 In the event of a program cancelation, the control
automatically deactivates the coupling.
402
DIN Programming
4.29 Other G codes
Eccentric X G727
G727 is used to machine elliptical polygons.
The turning contours are programmed using separate turning cycles.
Machine and control must be specially prepared by the
machine tool builder for use of this cycle. Refer to your
machine manual.
Requirement:
 Software option Synchronizing Functions
Parameters
H
Activate coupling
 H=0: Deactivate coupling
 H=1: Activate coupling
Q
Reference spindle: Number of the spindle that is coupled
with the X axis (machine-dependent)
I
X travel +/-: Half of the superimposed X-axis movement
(radius value)
C
C position at Z start: C-axis angle of X travel
F
Maximum rapid traverse: Permissible rapid traverse for the
X axis while coupling is active
E
Form factor: Number of X travels with respect to one
spindle revolution
Z
Z start: Reference value for the parameter C
W
Delta C [°/mm Z]: Difference in C-axis angle with respect to
a distance of 1 mm in the Z axis
Please note while programming:
 Program a workpiece blank increased by the center
offset in the radius if you are using turning cycles that
are referenced to the workpiece-blank definition.
 Program a starting point increased by the center offset
in the radius if you are using turning cycles that are not
referenced to the workpiece-blank definition.
 Reduce the spindle speed if you increase the center
offset.
 Reduce the maximum rapid traverse F if you increase
the center offset.
 Use identical values for the parameter Q when activating
and deactivating the coupling.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
403
4.29 Other G codes
Programming sequence:




Position the cursor in the MACHINING program section
Program G727 with H=1 (activate coupling)
Program turning cycles
Program G727 with H=0 (deactivate coupling)
Please note when executing the program:
 When the coupling is activated, the control positions the
tool in the Z axis to the value of the parameter Z.
 In the event of a program cancelation, the control
automatically deactivates the coupling.
404
DIN Programming
4.30 Data input and data output
4.30 Data input and data output
"WINDOW"—Output window for variables
WINDOW (x) opens an output window with x lines. The window is
opened as a result of the first input/output. WINDOW (0) closes the
window.
Syntax:
WINDOW(line number) (0 <= line number <= 20)
The standard window comprises 3 lines. You do not need to program
it.
Beispiel:
...
N
1 WINDOW(8)
N
2 INPUT("query: ",#l1)
N
3 #l2=17*#l1
N
4 PRINT("result: ",#l1,"*17 = ",#l2)
...
"WINDOW"—Output file for variables
The command WINDOW (x,"filename") saves the PRINT instruction in
a file with the defined name and the extension .LOG, in the directory
"V:\nc_prog\". The file is overwritten when the WINDOW command is
run again.
Syntax:
WINDOW(line number,"filename")
Beispiel:
...
N
1 WINDOW(8)
N
2 INPUT("query: ",#l1)
N
3 #l2=17*#l1
N
4 PRINT("result: ",#l1,"*17 = ",#l2)
...
"INPUT"—Input of variables
Use INPUT to program the input of variables.
Syntax:
INPUT("text",variable)
You define the input text and the number of the variable. The
Steuerung stops the interpretation at INPUT, outputs the text and
waits for input of the variable value. Instead of an input text, you can
also program a string variable, such as #x1.
The Steuerung displays the input after having completed the INPUT
command.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
405
4.30 Data input and data output
"PRINT"—Output of # variables
PRINT can be used to output texts and variable values during program
run. You can program a succession of several texts and variables.
Syntax:
PRINT("text",variable,"text",variable, ..)
Example:
PRINT("result: ",#l1,"*17 = ",#l2)
406
DIN Programming
4.31 Programming variables
4.31 Programming variables
The Steuerung provides a variety of variable types.
Syntax
Operator functions
The following rules apply to the use of variables:
+
Addition
–
Subtraction
*
Multiplication
/
Division
()
Parenthesizing
=
Equate function
Syntax
Arithmetic functions
ABS(...)
Absolute amount
ROUND(...)
Round
SQRT(...)
Square root
SQRTA(.., ..)
Square root of (a2+b2)
SQRTS(.., ..)
Square root of (a2–b2)
INT(...)
Truncate decimal places
Syntax
Trigonometric functions
SIN(...)
Sine (in degrees)
COS(...)
Cosine (in degrees)
TAN(...)
Tangent (in degrees)
ASIN(...)
Arc sine (in degrees)
ACOS(...)
Arc cosine (in degrees)
ATAN(...)
Arc tangent (in degrees)
Syntax
Other functions
LOGN(...)
Natural logarithm
EXP(...)
Exponential function ex
BITSET(...)
Bitset function
STRING(...)
String
PARA(...)
Configuration data
 Multiplication/division before addition/subtraction
 Up to 6 bracket levels
 Integer variables: Integer values between –32767 and +32768
 Real variables: Floating point numbers with max. 10 integers and 7
decimal places
 Do not use any blank spaces when programming variables.
 The variable number itself and an index value, if applicable, can be
described by another variable, e.g.: #g( #c2)
 See the table for the available functions
 The distinction made by CNCPILOT XXXX and
MANUALplus X110 controls between variables that can
be modified at runtime and those that cannot, does not
apply any longer. The NC program is no longer compiled
before the program run, but at runtime.
 Program NC blocks containing variable calculations with
"slide code $.." if your lathe has more than one slide.
Otherwise, the calculations are repeated.
 Positions and dimensions transferred into system
variables are always indicated in metric form. This also
applies when an NC program is run in inches.
You can also program the listed functions by soft key.
The soft-key row is available when the variable
assignment function is active and the alphabetic keyboard
is closed.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
407
4.31 Programming variables
Variable types
The Steuerung distinguishes the following variable types:
Beispiel:
General variables
...
 #l1 .. #l30 Channel-independent, local variables are effective
within a main or a subprogram.
 #c1 .. #c30 Channel-dependent, global variables can be used for
each slide (NC channel). Identical variable numbers on different
slides are no problem. The variable content is provided globally by
one channel; globally means that a variable described in a
subprogram can be evaluated in the main program, and vice versa.
 #g1 .. #g199 Channel-independent, global REAL variables are
provided once within the control. If the NC program changes a
variable, it applies to all slides. The variables are retained even when
the control is switched off, and can be evaluated again after powerup.
 #g200 .. #g299 Channel-independent, global INTEGER variables
are provided once within the control. If the NC program changes a
variable, it applies to all slides. The variables are retained even when
the control is switched off, and can be evaluated again after powerup.
 #x1 .. #x20 Channel-dependent, local text variables are effective
within a main or subprogram. They can only be read on the channel
to which they were written.
N.. #l1=#l1+1
N.. G1 X#c1
N.. G1 X(SQRT(3*(SIN(30)))
N.. #g1=(ABS(#2+0.5))
...
N.. G1 Z#m(#l1)(Z)
N.. #x1="Text"
N.. #g2=#g1+#l1*(27/9*3.1415)
...
If the variables are to be retained in the memory when the
control is switched off, this feature must be activated by
the machine tool builder (configuration parameter:
"Channels/ChannelSettings/CH_NC1/CfgNcPgmParState/
persistent=TRUE").
If this feature is not activated, the variables values will
always be "zero" after power-up.
Machine dimensions
 #m1(n) .. #m99(n): "n" is the designation of the axis (X, Z, Y) for
which the machine dimension is to be read or written. The variable
calculation uses the table "mach_dim.hmd".
Simulation: During the startup of the control, the table
"mach_dim.hmd" is read by the simulation. The simulation function
now uses the table of the simulation.
Beispiel: Machine dimensions
...
N.. G1 X(#m1(X)*2)
N.. G1 Z#m3(Z)
N.. #m4(Z)=350
...
408
DIN Programming
 #dt(n): "n" is the compensation direction (X, Z, Y, S) and "t" is the
turret pocket number assigned to the tool. The variable calculation
uses the table "toolturn.htt".
Simulation: When the program is selected, the table "toolturn.htt"
is read by the simulation. The simulation function now uses the table
of the simulation.
Beispiel: Tool compensation
...
N.. #d3(X)=0
N.. #d3(Z)=0.1
N.. #d3(S)=0.1
...
Tool information can also be interrogated directly via the ID
number. This may be necessary, for example, if no turret
pocket has been assigned. For this purpose, program a
comma and the ID number of the tool after the desired
identification, e.g. #l1 = #d1(Z, "001").
Event bits: Variable programming interrogates a bit of the event for 0
or 1. The meaning of the event is determined by the machine
manufacturer.
 #en(key): "n" is the channel number and "key" is the event name.
Used for reading external events set by the PLC.
 #e0(key[n].xxx): "n" is the channel number, "key" is the event name,
and "xxx" is the name extension. Used for reading external events
set by the PLC.
Beispiel: Events
...
N.. #g1 = #e1( "NP_DG_Achs_Modul_warten")
N.. PRINT( "NP_DG_Achs_Modul_warten
=",#g1)
N.. #g2 = #e1( "DG_DATEN[1]")
N.. PRINT( "DG_DATEN[1] =",#g2)
N.. #g3 = #e1( "SPI[1].DG_TEST[1]")
N.. PRINT( "SPI[1].DG_TEST[1] =",#g3)
...
N.. IF #e1( "NP_DG_Achs_Modul_warten")==4
N.. THEN
N.. G0 X40 Z40
N.. ELSE
N.. G0 X60 Z60
N.. ENDIF
...
HEIDENHAIN MANUALplus 620, CNC PILOT 640
409
4.31 Programming variables
Tool compensation
4.31 Programming variables
Reading tool data
Use the following syntax to read tool data. You can only access tools
that are entered in the turret list.
If a sequence of exchange is defined, program the first tool of the
sequence. The Steuerung determines the data of the active tool.
Tool information can also be interrogated directly via the ID
number. This may be necessary, for example, if no turret
pocket has been assigned. For this purpose, program a
comma and the ID number of the tool after the desired
identification, e.g. #l1 = #w1(Z, "001").
If you only need information on the current tool, it is
sufficient to program #w0(select).
Access to tool data of turret
Syntax:
 n = turret pocket number
 n = 0 for the current tool
 select = designates the information to
be read
Main machining direction
#wn(HR)
Tool ID number (assign in text variable (#xn))
#wn(PT)
P key of the tool *10 (e.g.: 12.3 becomes 123)
#wn(WT)
Tool type (3-digit number)
#wn(WTV)
1st position of tool type
Primary machining directions:
 0: Undefined
 1: +Z
 2: +X
 3: –Z
 4: –X
 5: +/–Z
 6: +/–X
Identification codes for tool information
#wn(ID)
#wn(select)
Execution
#wn(WTH) 2nd position of tool type
#wn(AS)
Versions
#wn(WTL)
3rd position of tool type
#wn(NL)
Usable length (inside turning and drilling tools)
#wn(HR)
Main machining direction (see table at right)
Tool orientation
#wn(NR)
Secondary machining direction of turning tools
#wn(WL)
#wn(AS)
Execution (see at right)
#wn(ZZ)
Number of teeth (milling tools)
#wn(RS)
Cutting edge radius
#wn(ZD)
Stud diameter
#wn(DF)
Cutter diameter
#wn(SD)
Shank diameter
#wn(SB)
Cutting width
#wn(SL)
Tooth length
#wn(AL)
Length of first cut
#wn(FB)
Cutter width
#wn(WL)
Tool orientation
410
 1: Right-hand
 2: Left-hand
Tool orientation (reference: machining
direction of tool):
 0: On the contour
 1: To the right of the contour
 – 1: To the left of the contour
DIN Programming
4.31 Programming variables
Identification codes for tool information
#wn(ZL)
Tool setting dimension in Z (from tool list)
#wn(XL)
Tool setting dimension in X (from tool list)
#wn(YL)
Tool setting dimension in Y (from tool list)
#wn(TL)
Tool status (tool locked)
#wn(I)
Position of tool tip center in X (see illustration)
#wn(J)
Position of tool tip center in Y
#wn(K)
Position of tool tip center in Z (see illustration)
#wn(ZE)
Length of the tool in the current insert position:
Distance between tool tip and slide zero point Z
#wn(XE)
Length of the tool in the current insert position:
Distance between tool tip and slide zero point X
#wn(YE)
Length of the tool in the current insert position:
Distance between tool tip and slide zero point Y
#wn(DN)
Diameter of drilling and milling tools
#wn(HW)
Principal angle in the normalized system (0° to 360°)
#wn(NW)
Secondary angle in the normalized system (0° to 360°)
#wn(EW)
Tool angle
#wn(SW)
Point angle
#wn(AW)
 0: No driven tool
 1: Driven tool
#wn(MD)
Direction of rotation:
 3: M3
 4: M4
#wn(CW)
Tilting plane angle
#wn(BW)
Angular offset
#wn(WTL)
Orientation
#wn(AC)
Cutting-edge insert angle
#wn(ZS)
Maximum cutting depth
#wn(GH)
Thread pitch
#wn(NE)
Number of secondary cutting edges
#wn(NS)
Number of the secondary cutting edge
HEIDENHAIN MANUALplus 620, CNC PILOT 640
411
4.31 Programming variables
Identification codes for tool information
#wn(FP)
Tool type: 0 = normal tool, 1 = master tools, 2 =
secondary cutting edge
#wn(Q)
Number of tool spindle
#wn(AS)
Execution left/right
#wn(X)
Setting dimension of holder in X
#wn(Z)
Setting dimension of holder in Z
#wn(Y)
Setting dimension of holder in Y
#wn(DX)
Compensation in X
#wn(DY)
Compensation in Y
#wn(DZ)
Compensation in Z
#wn(DS)
2nd compensation
412
DIN Programming
Use the following syntax to read diagnostic bits. You can access tools
that are entered in the turret list.
You can also read diagnostic bits for multifix tools. For this
purpose, program a comma and the ID number of the tool
after the desired identification code, e.g. #l1 = #t( 3,
"001").
Access to turret data
Syntax:
#tn(select)
 n = turret pocket number
 n = 0 for the current tool
 select = designates the information to
be read
Identification codes for diagnostic bits
#tn(1)
Tool life expired/workpiece quantity reached
#tn(2)
Breakage according to load monitoring (limit 2
exceeded)
#tn(3)
Wear according to load monitoring (limit 1 exceeded)
#tn(4)
Wear according to load monitoring (total load limit)
#tn(5)
Wear determined by tool measurement
#tn(6)
Wear determined by in-process measurement of
workpiece
#tn(7)
Wear determined by post-process measurement of
workpiece
#tn(8)
Cutting edge new =1 / used = 0
HEIDENHAIN MANUALplus 620, CNC PILOT 640
413
4.31 Programming variables
Reading diagnostic bits
4.31 Programming variables
Reading the current NC information
Use the following syntax to read NC information that was
programmed with G codes.
Identification codes for NC information
Access to current NC information
Syntax:
#nx(select)
 x = G-code number
 select = designates the information
to be read
#n0(X)
Last programmed position X
#n0(Y)
Last programmed position Y
#n0(Z)
Last programmed position Z
#n0(A)
Last programmed position A
#n0(B)
Last programmed position B
#n0(C)
Last programmed position C
#n0(U)
Last programmed position U
#n0(V)
Last programmed position V
Active wear compensation
#n0(W)
Last programmed position W
#n148(O)
#n0(CW)
Tool insert angle (0 or 180 degrees)
#n40(G)
Status of TRC (see table at right)
#n148(O)
Active wear compensation (see table at right)
#n18(G)
Active working plane (see table at right)
#n120(X)
Reference diameter X for calculating CY
#n52(G)
Oversize G52_Geo taken into account 0=no / 1=yes
#n57(X)
Oversize in X
#n57(Z)
Oversize in Z
Pocket data of entered tool
#n58(P)
Equidistant oversize
#n601(n)
#n150(X)
Cutting width shifted in X by G150/G151
#n150(Z)
Cutting width shifted in Z by G150/G151
#n95(G)
Programmed feed type (G93/G94/G95)
#n95(Q)
Spindle number of the last programmed feed rate
#n95(F)
Last programmed feed rate
#n97(G)
Programmed speed type (G96/G97)
#n97(Q)
Spindle number of the last programmed speed type
#n97(S)
Last programmed speed
Status of TRC
#n40(G)
TRC/MCRC status:
 40: G40 active
 41: G41 active
 42: G42 active
Active wear compensation (G148):
 0: DX, DZ
 1: DS, DZ
 2: DX, DS
Active working plane
414
#n18(G)
Active working plane:
 17: XY plane (front or rear face)
 18: XZ plane (turning view)
 19: YZ plane (plan view/surface)
Output in the format "SMppp":
 S: Tool edge number
 M: Magazine number
 ppp: Pocket number
DIN Programming
4.31 Programming variables
Identification codes for NC information
#n47(P)
Current safety clearance
#n147(I)
Current safety clearance in working plane
#n147(K)
Current safety clearance in infeed direction
#n601(n)
Pocket data of the tool entered in the magazine table
(see table at right)
#n610(H)
Next free magazine pocket (see table at right)
#n707(n, 1)
Read minimum value of software limit switch of axis
(see table at right)
#n707(n, 2)
Read maximum value of software limit switch of axis
(see table at right)
#n922(C)
Insert angle of cutting edge (for B axis)
#n922(H)
Mirroring status of cutting edge (0 = normal position,
1 = 180 degrees)
#n927(X)
Result of conversion function G927 for tool length in
X (for B axis)
#n927(Z)
Result of conversion function G927 for tool length in
Z (for B axis)
#n927(Y)
Result of conversion function G927 for tool length in
Y (for B axis)
#n995(H)
Query of current zone number for load monitoring
Free magazine pocket
#n610(H)
Output in the format "Mppp":
 M: Magazine number
 ppp: Pocket number
Software limit switches
#n707(n,1)
Identification code of axis:
 n: Axis X, Y, Z, U, V or W
 1: Minimum value
 2: Maximum value
HEIDENHAIN MANUALplus 620, CNC PILOT 640
415
4.31 Programming variables
Reading general NC information
Use the following syntax to read general NC information.
Identification codes for tool information
#i1
Active operating mode (see table at right)
#i2
Active unit of measure (inches/metric)
#i3
 Main spindle = 0
 Counterspindle with mirroring Z = 1
 Tool mirroring in Z = 2
 Tool + path mirroring in Z = 3
Active operating mode
#i1
 2: Machine tool
 3: Simulation
 5: TSF menu
Active unit of measure
#i2
Active unit of measure:
 0: Metric [mm]
 1: Inches [in]
#i4
G16 active = 1 (currently not used)
#i5
Last programmed T number
#i6
Start block search active = 1
Languages
#i7
System is DataPilot = 1
#i8
#i8
Selected language
#i9
If Y axis is configured = 1
#i10
If B axis is configured = 1
#i11
If the tool pocket in X is mirrored to the machine
system = 1
#i12
If U axis is programmable = 1
#i13
If V axis is programmable = 1
#i14
If W axis is programmable = 1
#i15
If U axis is configured = 1
#i16
If V axis is configured = 1
#i17
If W axis is configured = 1
#i18
Zero point shift of the Z axis
#i19
Zero point shift of the X axis
#i20
Last programmed path function (G0, G1, G2...)
#i21
Current quantity (workpiece counter)
#i22
If U axis is coupled with X axis = 1
#i23
If V axis is coupled with Y axis = 1
#i24
If W axis is coupled with Z axis = 1
#i25
If magazine exists = 1
416
Active operating mode:
Available languages:
 0: ENGLISH
 1: GERMAN
 2: CZECH
 3: FRENCH
 4: ITALIAN
 5: SPANISH
 6: PORTUGUESE
 7: SWEDISH
 8: DANISH
 9: FINNISH
 10: DUTCH
 11: POLISH
 12: HUNGARIAN
 14: RUSSIAN
 15: CHINESE
 16: CHINESE_TRAD
 17: SLOVENIAN
 19: KOREAN
 21: NORWEGIAN
 22: ROMANIAN
 23: SLOVAK
 24: TURKISH
DIN Programming
4.31 Programming variables
Identification codes for tool information
#i26
P key of actual tool *10 from tool preselection
#i27
P key of desired tool *10 from tool preselection
#i28
Angle of Y wedge axis
#i29
P key of the tool *10 that has reached the maximum
tool life
#i30
P key of the tool *10 that has reached the maximum
workpiece quantity
#i99
Return code of subprograms
HEIDENHAIN MANUALplus 620, CNC PILOT 640
417
4.31 Programming variables
Reading configuration data—PARA
The PARA function is used to read configuration data. To do this, use
the parameter designations from the configuration parameters. You
also use the designations from the configuration parameters to read
user parameters.
Access to configuration data
Syntax:
PARA(key, entity, attribute, index)
 Key: Keyword
 Entity: Name of the configuration
group
 Attribute: Element name
 Index: Array number if the attribute is
from an array
When you read optional parameters, check whether the return value
is valid. Depending on the data type of the parameter (REAL/STRING),
the value "0" or the text "_EMPTY" is returned when reading an optional
attribute that has not been set.
Example: PARA function
...
N.. #l10=PARA("","CfgDisplayLanguage","ncLanguage")
Reads the number of the currently selected
language
N.. #l1=PARA("","CfgGlobalTechPara","safetyDistWorkpOut")
Reads the external safety clearance on the
machined part (SAT)
N.. #l1=PARA("Z1","CfgAxisProperties","threadSafetyDist")
Reads the thread safety clearance for Z1
N.. #l1=PARA("","CfgCoordSystem","coordSystem")
Reads the machine orientation number
...
#x2=PARA("#x30","CfgCAxisProperties","relatedWpSpindle",0)
Check whether the optional parameter is set
IF #x2<>"_EMPTY"
Evaluation:
THEN
[ The parameter "relatedWpSpindle" was set ]
ELSE
[ The parameter "relatedWpSpindle" was not set ]
ENDIF
418
DIN Programming
You activate the index search for an element by appending the name
of the list element to the attribute, separated by a comma.
Access to configuration data
Example:
Syntax:
Determining the logical axis number of spindle S1
#c1 = PARA( "", "CfgAxes", "axisList,S1", 0)
The function returns the index of the "S1" element in the "axisList"
attribute of the "CfgAxes" entity. The index of element S1 equals the
logical axis number in this example.
Without the attribute extension "S1", the function would
read the element located at the list index number 0. Since
the element is a string in this example, the result has to be
assigned to a string variable.
PARA("key","entity","attribute,elem
ent", index)
 Key: Keyword
 Entity: Name of the configuration
group
 Attribute,name: Attribute name and
element name
 Index: 0 (not required)
#x1 = PARA( "", "CfgAxes", "axisList", 0)
The function reads the string name of the element at list
index number 0.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
419
4.31 Programming variables
Determining the index of a parameter element—
PARA
4.31 Programming variables
Expanded variable syntax CONST – VAR
By defining the key words CONST or VAR, you can assign names to
variables. The key words can be used in the main program and
subprogram. To use the definitions in a subprogram, you need to
declare the constant or variable before the MACHINING section code.
Rules for defining constants and variables:
The names of constants and variables must be preceded by an
underscore. They can comprise lower case letters, numbers and the
underscore character. The maximum length must not exceed 20
characters.
Variable names with VAR
By assigning variable names, you make it easier to read an NC
program. To do this, you must insert the program section VAR. In this
program section, you assign the variable designations to the variables.
Beispiel: Free-text variables
%abc.nc
VAR
#_rohdm=#l1 [#_rohdm is a synonym of #l1]
BLANK
N..
FINISHED
N..
MACHINING
N..
...
Beispiel: Subprogram
%SP1.ncS
VAR
#_wo = #c1
[tool orientation]
MACHINING
N.. #_wo = #w0(WTL)
N.. G0 X(#_posx*2)
N.. G0 X#_start_x
...
420
DIN Programming
 Direct assignment of values
 Internal interpreter information as constants
 Assignment of names to the transfer variables of subprograms
Use the following internal information to define constants in the
CONST section.
4.31 Programming variables
Definition of constants—CONST
Possibilities of defining constants:
Beispiel: Main program
%abc.nc
CONST
_square_root2 = 1.414213 [direct value
assignment]
Internal information for defining constants
_square_root_2 = SQRT(2) [direct value
assignment]
__n0_x
768 Last programmed position X
_posx = __n0_x
__n0_y
769 Last programmed position Y
__n0_z
770 Last programmed position Z
__n0_c
771 Last programmed position C
N..
__n40_g
774 Status of TRC
FINISHED
__n148_o
776 Active wear compensation
__n18_g
778 Active working plane
N..
__n120_x
787 Reference diameter X for calculating CY
...
__n52_g
790 Oversize G52_Geo taken into account 0=no /
1=yes
__n57_x
791 Oversize in X
__n57_z
792 Oversize in Z
__n58_p
793 Equidistant oversize
_posx = __n0_x
__n150_x
794 Cutting width shifted in X by G150/G151
VAR
__n150_z
795 Cutting width shifted in Z by G150/G151
__n95_g
799 Programmed feed type _G93/G94/G95)
N.. #_wo = #w0(WTL)
__n95_q
796 Spindle number of the programmed feed rate
N.. G0 X(#_posx*2)
__n95_f
800 Last programmed feed rate
N.. G0 X#_start_x
__n97_g
Programmed speed type _G96/G97)
__n97_q
797 Spindle number of the programmed speed type
__n97_s
Last programmed speed
__la-__z
Subprogram transfer values
[internal information]
VAR
...
BLANK
N..
MACHINING
Beispiel: Subprogram
%SP1.ncS
CONST
_start_x=__la [subprogram transfer value]
#_wo = #c1
[internal constant]
[tool orientation]
MACHINING
...
The constant "_pi" is predefined to the value
3.1415926535989 and can be used directly in every NC
program.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
421
4.32 Conditional block run
4.32 Conditional block run
Program branching IF..THEN..ELSE..ENDIF
A conditional branch consists of the elements:
 IF, followed by a condition. The condition includes a variable or
mathematical expression on either side of the relational operator.
 THEN. If the condition is fulfilled, the THEN branch is executed.
 ELSE. If the condition is not fulfilled, the ELSE branch is executed.
 ENDIF concludes the conditional program branch.
Interrogate bitset: You can also use the BITSET function as
condition. The function returns 1 if the numerical value contains the
requested bit. The function returns 0 if the numerical value does not
contain the requested bit.
Syntax: BITSET (x,y)
 x: Bit number (0 to 15)
 y: Numerical value (0 to 65535)
The relationship between bit number and numerical value is shown in
the table at right. You can also use variables for x, y.
Relational operators
<
Less than
<=
Less than or equal to
<>
Not equal to
>
Greater than
>=
Greater than or equal to
==
Equal to
Combining conditions:
AND
Logical AND operation
OR
Logical OR operation
0
which means
numerical
value
1
8
which means
numerical
value
256
1
2
9
512
2
4
10
1024
3
8
11
2048
4
16
12
4096
5
32
13
8192
6
64
14
16384
7
128
15
32768
Bit
Programming:





Select "Extras > DINplus word...". The Steuerung opens the "Insert
DIN PLUS word" selection list.
Select IF.
Enter the condition.
Insert NC blocks of the THEN branch.
If required: Insert NC blocks of the ELSE branch.
 NC blocks with IF, THEN, ELSE, ENDIF can have no
further commands.
 You can combine up to two conditions.
Bit
Beispiel: IF..THEN..ELSE..ENDIF
N.. IF (#l1==1) AND (#g250>50)
N.. THEN
N..
G0 X100 Z100
N.. ELSE
N..
G0 X0 Z0
N.. ENDIF
...
N.. IF 1==BITSET(0,#l1)
N.. THEN
N..
PRINT("Bit 0: OK")
...
422
DIN Programming
4.32 Conditional block run
Requesting variables and constants
With the DEF, NDEF, and DVDEF elements you can inquire whether a
valid value was assigned to a variable or a constant. For example, an
undefined variable can return the value 0, just like a variable that has
been assigned the value 0. You can prevent undesired program jumps
by examining the variables.
Programming:




Select "Extras > DINplus word...". The Steuerung opens the "Insert
DIN PLUS word" selection list
Select the IF command
Enter the required inquiry element (DEF, NDEF or DVDEF)
Enter the name of a variable or a constant
Beispiel: Requesting variable in subprogram
N.. IF DEF(__la)
N.. THEN
N.. PRINT("Value:",#__la)
N.. ELSE
N.. PRINT("#__la is not defined")
N.. ENDIF
...
Beispiel: Requesting variable in subprogram
Enter the variable name without the character "#", e.g. IF
NDEF(__la).
N.. IF NDEF(__lb)
N.. THEN
Inquiry elements of variables and constants:
 DEF: A value is assigned to a variable or constant
 NDEF: No value is assigned to a variable or constant
 DVDEF: Query of an internal constant
N.. PRINT("#__lb is not defined")
N.. ELSE
N.. PRINT("Value:",#__lb)
N.. ENDIF
...
Beispiel: Requesting constants
N.. IF DVDEF(__n97_s)
N.. THEN
N.. PRINT("__n97_s is defined",#__n97_s)
N.. ELSE
N.. PRINT("#__n97_s is not defined")
N.. ENDIF
...
HEIDENHAIN MANUALplus 620, CNC PILOT 640
423
4.32 Conditional block run
WHILE..ENDWHILE program repeat
A program repeat consists of the elements:
 WHILE, followed by a condition. The condition includes a variable or
mathematical expression on either side of the relational operator.
 ENDWHILE concludes the conditional program repeat.
NC blocks programmed between WHILE and ENDWHILE are
executed repeatedly for as long as the condition is fulfilled. If the
condition is not fulfilled, the Steuerung continues execution of the
program with the block programmed after ENDWHILE.
Interrogate bitset: You can also use the BITSET function as
condition. The function returns 1 if the numerical value contains the
requested bit. The function returns 0 if the numerical value does not
contain the requested bit.
Relational operators
<
Less than
<=
Less than or equal to
<>
Not equal to
>
Greater than
>=
Greater than or equal to
==
Equal to
Combining conditions:
Syntax: BITSET (x,y)
 x: Bit number (0 to 15)
 y: Numerical value (0 to 65535)
AND
Logical AND operation
OR
Logical OR operation
The relationship between bit number and numerical value is shown in
the table at right. You can also use variables for x, y.
Programming:




Select "Extras > DINplus word...". The Steuerung opens the "Insert
DIN PLUS word" selection list.
Select WHILE.
Enter the condition.
Insert NC blocks between WHILE and ENDWHILE.
 You can combine up to two conditions.
 If the condition you program in the WHILE command is
always true, the program remains in an endless loop.
This is one of the most frequent causes of error when
working with program repeats.
Bit
which means
numerical
value
Bit
which means
numerical
value
0
1
8
256
1
2
9
512
2
4
10
1024
3
8
11
2048
4
16
12
4096
5
32
13
8192
6
64
14
16384
7
128
15
32768
Beispiel: WHILE..ENDWHILE
...
N.. WHILE (#l4<10) AND (#l5>=0)
N..
G0 Xi10
...
N.. ENDWHILE
...
424
DIN Programming
4.32 Conditional block run
SWITCH..CASE—program branching
The switch statement consists of the elements:
 SWITCH, followed by a variable. The content of the variable is
interrogated in the following CASE statement.
 CASE x: The CASE branch is run with the variable value x. CASE can
be programmed repeated times.
 DEFAULT: This branch is executed if no CASE statement matched
the variable value. DEFAULT can be omitted.
 BREAK: Concludes the CASE branch or DEFAULT branch.
Programming:





Select "Extras > DINplus word...". The Steuerung opens the "Insert
DIN PLUS word" selection list.
Select SWITCH.
Enter the switch variable.
For each CASE branch:
 Select CASE (in "Extras > DINplus word...").
 Enter the SWITCH condition (value of the variable) and
Insert the NC blocks to be executed.
For the DEFAULT branch: Insert the NC blocks to be executed.
Example: SWITCH..CASE
...
N.. SWITCH #g201
N..
N..
CASE 1
[executed if #g201=1]
Executed if #g201=1
[executed if #g201=2]
Executed if #g201=2
G0 Xi10
...
N..
BREAK
N..
CASE 2
N..
G0 Xi20
...
N..
BREAK
N..
DEFAULT
N..
G0 Xi30
No CASE statement matched the variable value
...
N..
BREAK
N..
ENDSWITCH
...
HEIDENHAIN MANUALplus 620, CNC PILOT 640
425
4.32 Conditional block run
Skip level
In the Program Run submode, you can set/activate skip levels. The
next time the program is executed, the NC blocks defined by the set/
activated skip level will not be executed by the control (see User's
Manual).
Before you can set/activate skip levels, you need to define them in the
program:
Open the program in the smart.Turn operating mode.
Position the cursor in the MACHINING program section on the NC
block to be skipped.
Select "Skip level..." in the Extras menu.
Enter the number of the skip level in the "Deletion" parameter and
press the OK soft key to confirm.
You can assign more than one skip level to an NC block by
entering a string of numerals in the "Deletion" parameter.
The entry "159" corresponds to the skip levels 1, 5 and 9.
To clear the defined skip levels, program the parameter
without a value and press the OK soft key to confirm.
426
DIN Programming
4.33 Subprograms
4.33 Subprograms
Subprogram call: L"xx" V1
The subprogram contains the following elements:
 L: Identification letter for subprogram call
 "xx": Name of the subprogram—file name for external subprograms
(max. 16 letters or numbers)
 V1: Identification code for external subprograms—omitted for local
subprograms
Note on using subprograms:
 External subprograms are defined in a separate file. They can be
called from any main program or other subprogram.
 Local subprograms are in the main program file. They can be called
only from the main program.
 Subprograms can be nested up to 6 times. Nesting means that
another subprogram is called from within a subprogram.
 Recursion should be avoided.
 You can program up to 29 transfer values in a subprogram call.
 Designations: LA to LF, LH, I, J, K, O, P, R, S, U, W, X, Y, Z, BS,
BE, WS, AC, WC, RC, IC, KC and JC
 The identification code within the subprogram is "#__..", followed
by the parameter designation in lowercase letters (for example:
#__la).
 Use the transfer values when programming with variables within
the subprogram.
 String variables: ID and AT
 The variables #l1 – #l30 are available in every subprogram as local
variables.
 To transfer a variable to the main program, program the variable
after the fixed word RETURN. In the main program, the information
is available in #i99.
 If a subprogram is to be executed repeatedly, define in the "number
of repeats" Q parameter the number of times the subprogram is to
be repeated.
 A subprogram ends with RETURN.
The parameter LN is reserved for the transfer of block
numbers. This parameter may receive a new value when
the NC program is renumbered.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
427
4.33 Subprograms
Dialog texts in subprogram call
You can define up to 30 parameter descriptions that precede/follow
the input fields in an external subprogram. The units of measure are
defined using code numbers. Depending on the setting "metric" or
"inches," the Steuerung shows the designations (of the units of
measure). When calling external subprograms that contain a
parameter list, then parameters not contained in this list are omitted
from the call dialog.
pn:
Parameter designations (la, lb, ...)
n:
Code number for units of measure
 0: Non-dimensional
 1: mm or inches
 2: mm/rev or inch/rev
 3: mm/min or inch/min
 4: m/min or ft/min
 5: Rev/min
 6: Degrees (°)
 7: µm or µinch
The parameter descriptions can be positioned within the subprogram
as desired. The control searches for subprograms in the sequence:
current project, standard directory and then machine manufacturer
directory.
Parameter descriptions (see table at right):
[//] – Beginning
[pn=n; s=parameter text (up to 25 characters) ]
Beispiel:
[//] – End
...
[//]
[la=1; s=bar diameter]
[lb=1; s=starting point in Z]
[lc=1; s=chamfer/rounding arc (-/+)]
...
[//]
...
428
DIN Programming
4.33 Subprograms
Help graphics for subprogram calls
With help graphics you illustrate the call parameters of subprograms.
The Steuerung places the help graphics to the left next to the dialog
box of the subprogram call.
If you append an underscore "_" and the input field name in capital
letters (beginning with L) to the name of the file, a separate graphic
will be displayed for that input field. If no separate help graphic exists
for an input field, the graphic for the subprogram will be displayed (if
available). By default, the help window is displayed only if there is a
graphic for the subprogram. Even if you want to use individual graphics
for the address letters, you should define a graphic for the
subprogram.
Graphic format:
 BMP, PNG, JPG images
 Size 440x320 pixels
You integrate help graphics for subprogram calls as follows:


The subprogram name, entry field name and the appropriate
extension (BMP, PNG, JPG) must be used as file name for the help
graphic.
Transfer the help graphic to the directory: \nc_prog\Pictures
HEIDENHAIN MANUALplus 620, CNC PILOT 640
429
4.34 M commands
4.34 M commands
M commands for program-run control
The effect of machine commands depends on the configuration of
your machine. On your lathe, other M commands may apply for the
listed functions. Refer to your machine manual.
Overview: M commands for program-run control
M00
Program stop
The program run stops. Cycle start resumes the
program run.
M01
Optional stop
If the Continuous run soft key is not active in
Automatic mode, the program run stops with M01.
Cycle start resumes the program run. If Continuous
run is active, the program continues without
stopping.
M18
Counting pulse
M30
End of program
M30 means "end of program" (you do not need to
program M30). If you press Cycle start after M30,
program execution is repeated from the start of the
program.
M417
Activate protection zone monitoring
M418
Deactivate protection zone monitoring
M99 NS..
Program end with restart
M99 means end program and start again. Steuerung
restarts program execution from:
 The start of program if no NS is entered
 The block number NS if a NS is entered
Modal functions (feed rate, spindle speed, tool number,
etc.) which are effective at the end of program remain in
effect when the program is restarted. You should
therefore reprogram the modal functions at the start of
program or at the startup block (if M99 is used).
430
DIN Programming
4.34 M commands
Machine commands
The effect of machine commands depends on the configuration of
your machine. The following table lists the M commands used on
most machines.
M commands as machine commands
M03
Main spindle on (cw)
M04
Main spindle on (ccw)
M05
Main spindle stop
M12
Lock main spindle brake
M13
Release main spindle brake
M14
C axis on
M15
C axis off
M19..
Spindle stop at position C
M40
Shift gear to range 0 (neutral)
M41
Shift gear to range 1
M42
Shift gear to range 2
M43
Shift gear to range 3
M44
Shift gear to range 4
Mx03
Spindle x on (cw)
Mx04
Spindle x on (ccw)
Mx05
Spindle x stop
For more information on the M commands, refer to your
machine manual.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
431
4.35 G codes from previous controls
4.35 G codes from previous controls
The commands described in the following are supported to enable you
to use NC programs from previous controls. HEIDENHAIN
recommends against using these commands in new NC programs.
Contour definitions in the machining section
Undercut contour G25
G25 generates an undercut form element (DIN 509 E, DIN 509 F,
DIN 76) that can be integrated in the contour description of roughing
or finishing cycles. The help graphic illustrates the undercut
parameters.
Parameters
H
Undercut type (default: 0)
I
K
R
P
W
A
FP
U
E
 H=0, 5: DIN 509 E
 H=6: DIN 509 F
 H=7: DIN 76
Undercut depth (default: value from standard table)
Undercut width (default: value from standard table)
Undercut radius (default: value from standard table)
Face depth (default: value from standard table)
Undercut angle (default: value from standard table)
Face angle (default: value from standard table)
Thread pitch—no value: Pitch calculated from thread diameter
Grinding oversize (default: 0)
Reduced feed for machining the undercut (default: active feed
rate)
If the parameters are not defined, the Steuerung determines the
following values from the diameter or the thread pitch in the standard
table:
 DIN 509 E: I, K, W, R
 DIN 509 F: I, K, W, R, P, A
 DIN 76: I, K, W, R (determined from the thread pitch)
432
DIN Programming
 All parameters that you enter will be accounted for—
even if the standard table prescribes other values.
 If you are programming an internal thread, it is advisable
to preset the thread pitch FP since the diameter of the
longitudinal element is not the thread diameter. If you
have the Steuerung calculate the thread pitch
automatically, slight deviations may occur.
4.35 G codes from previous controls
Beispiel: G25
%25.nc
[G25]
N1 T1 G95 F0.4 G96 S150 M3
N2 G0 X62 Z2
N3 G819 P4 H0 I0.3 K0.1
N4 G0 X13 Z0
N5 G1 X16 Z-1.5
N6 G1 Z-30
N7 G25 H7 I1.15 K5.2 R0.8 W30 FP1.5
N8 G1 X20
N9 G1 X40 Z-35
N10 G1 Z-55 B4
N11 G1 X55 B-2
N12 G1 Z-70
N13 G1 X60
N14 G80
END
HEIDENHAIN MANUALplus 620, CNC PILOT 640
433
4.35 G codes from previous controls
Simple turning cycles
Simple longitudinal roughing G81
G81 roughs the contour area defined by the current tool position and
X, Z. If you wish to machine an oblique cut, you can define the angle
with I and K.
Parameters
X
Starting point of contour in X (diameter value)
Z
Contour end point
I
Maximum infeed in X
K
Offset in Z direction (default: 0)
Q
G code for infeed (default: 0)
V
 0: Infeed with G0 (rapid traverse)
 1: Infeed with G1 (feed rate)
Type of retraction (default: 0)
H
 0: Return to cycle starting point in Z and last retraction
diameter in X
 1: Return to cycle starting point
Type of departure (default: 0)
 0: With each cut (machine contour outline after each pass)
 2: No smoothing (retracts at 45°; no contour smoothing)
The Steuerung uses the position of the target point to distinguish
between external and internal machining. The number of cutting
passes is calculated so that an abrasive cut is avoided and the
calculated infeed distance is <= I.
 Programming X, Z: Absolute, incremental or modal
 The tool radius compensation is not active.
 Safety clearance after each pass: 1 mm
 A G57 oversize
 Is calculated with algebraic sign (oversizes are
therefore impossible for inside contour machining)
 Remains effective after cycle end
 A G58 oversize is not taken into account.
Beispiel: G81
...
N1 T3 G95 F0.25 G96 S200 M3
N2 G0 X120 Z2
N3 G81 X100 Z-70 I4 K4 Q0
N4 G0 X100 Z2
N5 G81 X80 Z-60 I-4 K2 Q1
N6 G0 X80 Z2
N7 G81 X50 Z-45 I4 Q1
...
434
DIN Programming
4.35 G codes from previous controls
Simple face roughing G82
G82 roughs the contour area defined by the current tool position and
X, Z. If you wish to machine an oblique cut, you can define the angle
with I and K.
Parameters
X
Contour end point in X (diameter value)
Z
Contour starting point
I
Offset in X direction (default: 0)
K
Maximum infeed in Z
Q
G code for infeed (default: 0)
V
 0: Infeed with G0 (rapid traverse)
 1: Infeed with G1 (feed rate)
Type of retraction (default: 0)
H
 0: Return to cycle starting point in X and last retraction
position in Z
 1: Return to cycle starting point
Type of departure (default: 0)
 0: With each cut (machine contour outline after each pass)
 2: No smoothing (retracts at 45°; no contour smoothing)
The Steuerung uses the position of the target point to distinguish
between external and internal machining. The number of cutting
passes is calculated so that an abrasive cut is avoided and the
calculated infeed distance is <= K.
 Programming X, Z: Absolute, incremental or modal
 The tool radius compensation is not active.
 Safety clearance after each pass: 1mm
 A G57 oversize
 Is calculated with algebraic sign (oversizes are
therefore impossible for inside contour machining)
 Remains effective after cycle end
 A G58 oversize is not taken into account.
Beispiel: G82
...
N1 T3 G95 F0.25 G96 S200 M3
N2 G0 X120 Z2
N3 G82 X20 Z-15 I4 K4 Q0
N4 G0 X120 Z-15
N5 G82 X50 Z-26 I2 K-4 Q1
N6 G0 X120 Z-26
N7 G82 X80 Z-45 K4 Q1
...
HEIDENHAIN MANUALplus 620, CNC PILOT 640
435
4.35 G codes from previous controls
Simple contour repeat cycle G83
G83 carries out the functions programmed in the following blocks
(simple traverses or cycles without a contour definition) more than
once. G80 ends the machining cycle.
Parameters
X
Contour target point (diameter)—(default: Load the last X
coordinate)
Z
Contour target point (default: Load the last Z coordinate)
I
Maximum infeed in X direction (radius)—(default: 0)
K
Maximum infeed in Z direction (default: 0)
If the number of infeeds differs for the X and Z axes, the tool first
advances in both axes with the programmed values. The infeed is set
to zero if the target value for one direction is reached.
Programming:
 G83 is alone in the block
 G83 must not be nested, not even by calling subprograms
 The tool radius compensation is not active. You can
program the TRC separately with G40 to G42.
 Safety clearance after each pass: 1mm
 A G57 oversize
 Is calculated with algebraic sign (oversizes are
therefore impossible for inside contour machining)
 Remains effective after cycle end
 A G58 oversize
 Is taken into account if you work with TRC
 Remains effective after cycle end
Beispiel: G83
...
N1 T3 G95 F0.25 G96 S200 M3
N2 G0 X120 Z2
N3 G83 X80 Z0 I4 K0.3
N4 G0 X80 Z0
N5 G1 Z-15 B-1
N6 G1 X102 B2
N7 G1 Z-22
N8 G1 X90 Zi-12 B1
N9 G1 Zi-6
Danger of collision!
N10 G1 X100 A80 B-1
After each pass, the tool returns on a diagonal path before
it advances for the next pass. If required, program an
additional rapid traverse path to avoid a collision.
N11 G1 Z-47
N12 G1 X110
N13 G0 Z2
N14 G80
436
DIN Programming
4.35 G codes from previous controls
Recessing G86
G86 machines simple radial and axial recesses with chamfers. From
the tool position, the Steuerung determines whether a radial or axial
recess, or an inside or outside recess is to be machined.
Parameters
X
Base corner point (diameter)
Z
Base corner point
I
Radial recess: Oversize
 I>0: Oversize (roughing and finishing)
 I=0: No finishing
Axial recess: Recess width
K
 I>0: Recess width
 No input: Recess width = tool width
Radial recess: Recess width
 K>0: Recess width
 No input: Recess width = tool width
Axial recess: Oversize
E
 K>0: Oversize (roughing and finishing)
 K=0: No finishing
Dwell time (for chip breaking)—(default: length of time for one
revolution)
 With finishing oversize: Only for finishing
 Without finishing oversize: For every recess
"Oversize" programmed: First roughing, then finishing
Beispiel: G86
G86 machines chamfers at the sides of the recess. If you do not wish
to cut the chamfers, you must position the tool at a sufficient distance
from the workpiece. Calculate the starting position XS (diameter) as
follows:
...
XS = XK + 2 * (1.3 – b)
XK:
Contour diameter
b:
Chamfer width
N3 G86 X54 Z-30 I0.2 K7 E2 [radial]
 The tool radius compensation is active.
 Oversizes are not taken into account.
N1 T30 G95 F0.15 G96 S200 M3
N2 G0 X62 Z2
N4 G14 Q0
N5 T38 G95 F0.15 G96 S200 M3
N6 G0 X120 Z1
N7 G86 X102 Z-4 I7 K0.2 E1 [axial]
...
HEIDENHAIN MANUALplus 620, CNC PILOT 640
437
4.35 G codes from previous controls
Radius cycle G87
G87 machines transition radii at orthogonal, paraxial inside and outside
corners. The direction is taken from the position/machining direction
of the tool.
Parameters
X
Corner point (diameter)
Z
Corner point
B
Radius
E
Reduced feed rate (default: active feed)
A preceding longitudinal or transverse element is machined if the tool
is located at the X or Z coordinate of the corner before the cycle is
executed.
 The tool radius compensation is active.
 Oversizes are not taken into account.
Beispiel: G87
...
N1 T3 G95 F0.25 G96 S200 M3
N2 G0 X70 Z2
N3 G1 Z0
N4 G87 X84 Z0 B2 [radius]
Chamfer cycle G88
G88 machines chamfers at orthogonal, paraxial outside corners. The
direction is taken from the position/machining direction of the tool.
Parameters
X
Corner point (diameter)
Z
Corner point
B
Chamfer width
E
Reduced feed rate (default: active feed)
A preceding longitudinal or transverse element is machined if the tool
is located at the X or Z coordinate of the corner before the cycle is
executed.
 The tool radius compensation is active.
 Oversizes are not taken into account.
Beispiel: G88
...
N1 T3 G95 F0.25 G96 S200 M3
N2 G0 X70 Z2
N3 G1 Z0
N4 G88 X84 Z0 B2 [chamfer]
438
DIN Programming
4.35 G codes from previous controls
Thread cycles (4110)
Simple longitudinal single-start thread G350
G350 cuts a longitudinal thread (internal or external). The thread starts
at the current tool position and ends at the end point Z.
Parameters
Z
Corner point of thread
F
Thread pitch
U
Thread depth
I
 U>0: Internal thread
 U<0: External thread
 U=+999 or –999: Thread depth is calculated
Maximum infeed (no input: I is calculated from the thread pitch
and the thread depth)
Internal or external threads: See algebraic sign of "U."
Handwheel superposition (provided that your machine is equipped
accordingly): The superposition is limited to the following range:
 X direction: Depending on the current cutting depth without
exceeding the starting and end points of the thread.
 Z direction: Maximal 1 thread groove, without exceeding the
starting and end points of the thread.
 Cycle stop becomes effective at the end of a thread
cut.
 The feed rate and spindle speed overrides are not
effective during cycle run.
 Handwheel superimpositioning can be activated with a
switch located on the machine operating panel if your
machine is equipped accordingly.
 Feedforward control is switched off.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
439
4.35 G codes from previous controls
Simple longitudinal multi-start thread G351
G351 machines a single or multi-start longitudinal thread (internal or
external thread) with variable pitch. The thread starts at the current
tool position and ends at the end point Z.
Parameters
Z
Corner point of thread
F
Thread pitch
U
Thread depth
I
A
D
J
E
 U>0: Internal thread
 U<0: External thread
 U=+999 or –999: Thread depth is calculated
Maximum infeed (no input: I is calculated from the thread pitch
and the thread depth)
Approach angle (angle of infeed) (default: 30°; range: –
60°<A<60°)
 A>0: Infeed on right thread flank
 A<0: Infeed on left thread flank
Threads per unit (default: 1)
Remaining cutting depth (default: 1/100 mm)
Variable pitch (default: 0)
 E>0: Increases the pitch per revolution by E
 E<=: Decreases the pitch per revolution by E
Internal or external threads: See algebraic sign of "U."
Number of cutting passes: "I" is used for the first pass. The cutting
depth is reduced with each further pass until the "remaining cutting
depth J" is reached.
Handwheel superposition (provided that your machine is equipped
accordingly): The superposition is limited to the following range:
 X direction: Depending on the current cutting depth without
exceeding the starting and end points of the thread.
 Z direction: Maximal 1 thread groove, without exceeding the
starting and end points of the thread.
 Cycle stop becomes effective at the end of a thread
cut.
 The feed rate and spindle speed overrides are not
effective during cycle run.
 Handwheel superimpositioning can be activated with a
switch located on the machine operating panel if your
machine is equipped accordingly.
 Feedforward control is switched off.
440
DIN Programming
4.36 DINplus program example
4.36 DINplus program example
Example of a subprogram with contour
repetitions
Contour repetitions, including saving of the contour
HEADER
#SLIDE $1
TURRET 1
T2 ID "121-55-040.1"
T3 ID "111-55.080.1"
T4 ID "161-400.2"
T8 ID "342-18.0-70"
T12 ID "112-12-050.1"
BLANK
N1 G20 X100 Z120 K1
FINISHED
N2 G0 X19.2 Z-10
N3 G1 Z-8.5 BR0.35
N4 G1 X38 BR3
N5 G1 Z-3.05 BR0.2
N6 G1 X42 BR0.5
N7 G1 Z0 BR0.2
N8 G1 X66 BR0.5
N9 G1 Z-10 BR0.5
N10 G1 X19.2 BR0.5
MACHINING
N11 G26 S2500
N12 G14 Q0
N13 G702 Q0 H1
Save contour
N14 L"1" V0 Q2
Qx = number of repetitions
N15 M30
SUBPROGRAM "1"
N16 M108
N17 G702 Q1 H1
HEIDENHAIN MANUALplus 620, CNC PILOT 640
Load saved contour
441
4.36 DINplus program example
N18 G14 Q0
N19 T8
N20 G97 S2000 M3
N21 G95 F0.2
N22 G0 X0 Z4
N23 G147 K1
N24 G74 Z-15 P72 I8 B20 J36 E0.1 K0
N25 G14 Q0
N26 T3
N27 G96 S300 G95 F0.35 M4
N28 G0 X72 Z2
N29 G820 NS8 NE8 P2 K0.2 W270 V3
N30 G14 Q0
N31 T12
N32 G96 S250 G95 F0.22
N33 G810 NS7 NE3 P2 I0.2 K0.1 Z-12 H0 W180 Q0
N34 G14 Q2
N35 T2
N36 G96 S300 G95 F0.08
N37 G0 X69 Z2
N38 G47 P1
N39 G890 NS8 V3 H3 Z-40 D3
N40 G47 P1
N41 G890 NS9 V1 H0 Z-40 D1 I74 K0
N42 G14 Q0
N43 T12
N44 G0 X44 Z2
N45 G890 NS7 NE3
N46 G14 Q2
N47 T4
Insert parting tool
N48 G96 S160 G95 F0.18 M4
N49 G0 X72 Z-14
N50 G150
Shift reference point to the right of the cutting edge
N51 G1 X60
N52 G1 X72
N53 G0 Z-9
N54 G1 X66 G95 F0.18
N55 G42
442
Activate TRC
DIN Programming
4.36 DINplus program example
N56 G1 Z-10 B0.5
N57 G1 X17
N58 G0 X72
N59 G0 X80 Z-10 G40
Deactivate TRC
N60 G14 Q0
N61 G56 Z-14.4
Incremental zero point shift
RETURN
END
HEIDENHAIN MANUALplus 620, CNC PILOT 640
443
4.37 Connection between geometry and machining commands
4.37 Connection between geometry
and machining commands
Turning Operations
Function
Geometry
Machining
Individual elements
 G0..G3
 G12/G13
 G810 Longitudinal roughing cycle
 G820 Face roughing cycle
 G830 Contour-parallel roughing cycle
 G835 Contour-parallel with neutral tool
 G860 Universal recessing cycle
 G869 Recess turning cycle
 G890 Finishing cycle
Recess
 G22 (standard)
 G860 Universal recessing cycle
 G870 Simple recessing cycle
 G869 Recess turning cycle
Recess
 G23
 G860 Universal recessing cycle
 G869 Recess turning cycle
Thread with undercut
 G24
 G810 Longitudinal roughing cycle
 G820 Face roughing cycle
 G830 Contour-parallel roughing cycle
 G890 Finishing cycle
 G31 Thread cycle
Undercut
 G25
 G810 Longitudinal roughing cycle
 G890 Finishing cycle
Thread
 G34 (standard)
 G37 (general)
 G31Thread cycle
Hole
 G49 (turning center)
 G71 Simple drilling cycle
 G72 Boring, countersinking, etc.
 G73 Tapping cycle
 G74 Deep-hole drilling cycle
444
DIN Programming
4.37 Connection between geometry and machining commands
C-axis machining—front/rear face
Function
Geometry
Machining
Individual elements
 G100 to G103
 G840 Contour milling
 G845/G846 Pocket milling, roughing/finishing
Figures
 G301 Linear slot
 G302/G303 Circular slot
 G304 Full circle
 G305 Rectangle
 G307 Eccentric polygon
 G840 Contour milling
 G845/G846 Pocket milling, roughing/finishing
Hole
 G300
 G71 Simple drilling cycle
 G72 Boring, countersinking, etc.
 G73 Tapping cycle
 G74 Deep-hole drilling cycle
C-axis machining—lateral surface
Function
Geometry
Machining
Individual elements
 G110 to G113
 G840 Contour milling
 G845/G846 Pocket milling, roughing/finishing
Figures
 G311 Linear slot
 G312/G313 Circular slot
 G314 Full circle
 G315 Rectangle
 G317 Eccentric polygon
 G840 Contour milling
 G845/G846 Pocket milling, roughing/finishing
Hole
 G310
 G71 Simple drilling cycle
 G72 Boring, countersinking, etc.
 G73 Tapping cycle
 G74 Deep-hole drilling cycle
HEIDENHAIN MANUALplus 620, CNC PILOT 640
445
4.38 Full-surface machining
4.38 Full-surface machining
Fundamentals of full-surface machining
In "full-surface machining," the front and rear ends can be machined in
one NC program. The control supports full-surface machining for all
common machine designs. The features include angle-synchronous
part transfer with rotating spindle, traversing to a stop, controlled
parting, and coordinate transformation. This ensures efficient fullsurface machining and simple programming.
You describe the turning contour, the contours for the C axis as well
as full-surface machining functions in one NC program. Expert
programs are available for configuring the lathe.
You can also enjoy the benefits of full-surface machining on lathes
with only one spindle.
Rear-face contours with C axis: The XK axis and therefore also the
C axis are oriented with respect to the workpiece, not to the spindle.
Therefore, for the rear face:
 Orientation of the XK axis: To the left (front face: to the right)
 Orientation of the C axis: Clockwise
 Direction of rotation for circular arcs G102: Counterclockwise
 Direction of rotation for circular arcs G103: Clockwise
Turning: The control supports full-surface machining with conversion
and mirroring functions. This makes it possible to keep the usual
directions of movement for rear-side machining as well.
 Program a positive value to depart the workpiece
 Program a negative value to approach the workpiece.
The machine manufacturer can provide your lathe with suitable expert
programs for workpiece transfer.
Reference points and coordinate system: The position of the
machine and workpiece zero points as well as the coordinate systems
for the spindle and opposing spindle are illustrated in the figure at
bottom. With this design of lathe it is recommended to mirror only the
Z axis. Then, for either spindle, moving in positive direction will stand
for motion away from the workpiece.
Usually the expert program contains the mirroring of the Z axis and the
zero-point shift by the dimension "NP-Offs."
(Trans_Z1)
446
DIN Programming
4.38 Full-surface machining
Programming of full-surface machining
When programming a contour on the rear face, be sure to consider the
orientation of the XK axis (or X axis) and rotational direction of arcs.
Insofar as you use drilling and milling cycles, there are no special
aspects to rear-face machining, since these cycles refer to predefined
contours.
For rear-face machining with the basic commands G100 to G103 the
same conditions apply as for rear-face contours.
Turning: The expert programs for rechucking contain converting and
mirroring functions. The following principle applies for rear-face
machining (2nd setup):
 + direction: Goes away from the workpiece
 – direction: Goes toward the workpiece
 G2/G12: Circular arc clockwise
 G3/G13: Circular arc counterclockwise
Working without expert programs
If you do not use the expert programs or the converting and mirroring
functions, the following principle applies:
 + direction: Goes away from the main spindle
 – direction: Goes toward the main spindle
 G2/G12: Circular arc clockwise
 G3/G13: Circular arc counterclockwise
HEIDENHAIN MANUALplus 620, CNC PILOT 640
447
4.38 Full-surface machining
Full-surface machining with opposing spindle
G30: The expert program switches the kinematics of the
counterspindle. In addition, G30 activates the mirroring of the Z axis
and converts other functions (e.g. circular arcs G2, G3).
G99: The expert program shifts the contour and mirrors the coordinate
system (Z axis). Further programming of G99 is normally not required
for machining the rear face after rechucking.
Example: The workpiece is machined on the front face, transferred to
the opposing spindle through an expert program and machined on the
rear face (see illustrations).
The expert program is used for:
 Angle-synchronous workpiece transfer to the opposing spindle
 Mirroring traverse paths in the Z axis
 Activating a conversion list
 Mirroring the contour description and shifting for the 2nd setup
Full-surface machining on machines with opposing spindles
HEADER
#MATERIAL
#MEASURE_UNITS
STEEL
METRIC
TURRET
T1
ID "512-600.10"
T2
ID "111-80-080.1"
T102
ID "115-80-080.1"
BLANK
N1 G20 X100 Z100 K1
FINISHED
...
FACE_C Z0
N 13 G308 ID"Line" P-1
N 14
G100 XK-15 YK10
N 15
G101 XK-10 YK12 BR2
N 16
G101 XK-4.0725 YK-12.6555 BR4
N 18
G101 XK10
N 19 G309
REAR_C Z-98
...
MACHINING
448
DIN Programming
Zero point shift for 1st setup
N28 G0 W#iS18
Counterspindle to machining position
4.38 Full-surface machining
N27 G59 Z233
N30 G14 Q0
N31 G26 S2500
N32 T2
...
N63 M5
N64 T1
N65 G197 S1485 G193 F0.05 M103
C-axis machining in the main spindle
N66 M14
N67 M107
N68 G0 X36.0555 Z3
N69 G110 C146.31
N70 G147 I2 K2
N71 G840 Q0 NS15 NE18 I0.5 R0 P1
N72 G0 X31.241 Z3
N73 G14 Q0
N74 M105 M109
N76 M15
Deactivate C axis
N80 L"RECHUCK" V1 LA.. LB.. LC..
Expert prog. for part transfer with following
functions:
G720 Spindle synchronization
G916 Traversing to a fixed stop
G30 Switch the kinematics
G99 Mirroring and shifting of the workpiece
contour
N90 G59 Z222
Zero point shift for 2nd setup
...
N91 G14 Q0
N92 T102
N93 G396 S220 G395 F0.2 M304
Technology data for opposing spindle
N94 M107
Turning in the counterspindle
N95 G0 X120 Z3
N96 G810 ....
Fixed cycles
N97 G30 Q0
Switch off rear-face machining
...
N129 M30
END
HEIDENHAIN MANUALplus 620, CNC PILOT 640
449
4.38 Full-surface machining
Full-surface machining with single spindle
G30: Normally not required
G99: The expert program mirrors the contour. Further programming of
G99 is normally not required for machining the rear face after
rechucking.
Example: The front and rear face of the workpiece are machined using
one NC program. The workpiece is first machined on the front face;
then it is rechucked manually. The rear face is machined
subsequently.
The expert program mirrors and shifts the contour for the 2nd setup.
Full-surface machining on machine with one spindle
HEADER
#MATERIAL
#MEASURE_UNITS
STEEL
METRIC
TURRET
T1 ID "512-600.10"
T2 ID "111-80-080.1"
T4 ID "121-55-040.1"
BLANK
N1 G20 X100 Z100 K1
FINISHED
...
FACE_C Z0
...
REAR_C Z-98
N20 G308 ID"R" P-1
N21 G100 XK5 YK-10
N22 G101 YK15
N23 G101 XK-5
N24 G103 XK-8 YK3.8038 R6 I-5
N25 G101 XK-12 YK-10
N26 G309
MACHINING
450
DIN Programming
4.38 Full-surface machining
N27 G59 Z233
Zero point shift for 1st setup
...
N82 M15
Prepare the rechucking
N86 G99 H1 V0 K-98
Contour mirroring and shifting for manual
rechucking
N87 M0
Stop for rechucking
N88 G59 Z222
Zero point shift for 2nd setup
...
N125 M5
Milling – rear face
N126 T1
N127 G197 S1485 G193 F0.05 M103
N128 M14
N130 M107
N131 G0 X22.3607 Z3
N132 G110 C-116.565
N134 G147 I2 K2
N135 G840 Q0 NS22 NE25 I0.5 R0 P1
N136 G0 X154 Z-95
N137 G0 X154 Z3
N138 G14 Q0
N139 M105 M109
N142 M15
N143 G30 Q0
Switch off rear-face machining
N144 M30
END
HEIDENHAIN MANUALplus 620, CNC PILOT 640
451
452
DIN Programming
4.38 Full-surface machining
Touch probe cycles
5.1 General information on touch probe cycles (software option)
5.1 General information on touch
probe cycles (software option)
The control must be specially prepared by the machine
tool builder for the use of a 3-D touch probe. The machine
manual provides further information.
Please note that HEIDENHAIN grants a warranty for the
function of the touch probe cycles only if HEIDENHAIN
touch probes are used!
Principle of function of touch probe cycles
When you run a touch probe cycle, the 3-D touch probe is prepositioned at positioning feed rate. The actual probing movement is
then executed from there at probing feed rate. The machine tool
builder determines the positioning feed rate for the touch probe in a
machine parameter. You define the probing feed rate in the respective
touch probe cycle.
When the probe stylus contacts the workpiece,
 the 3-D touch probe transmits a signal to the control: the
coordinates of the probed position are stored,
 the touch probe stops moving, and
 returns to the starting position of the probing procedure at
positioning feed rate.
If the stylus is not deflected within a defined distance, the control
displays an error message.
454
Touch probe cycles
5.1 General information on touch probe cycles (software option)
Touch probe cycles for automatic operation
The control provides numerous touch probe cycles for various
applications:
 Calibrating a touch trigger probe
 Measuring circles, circle segments, angle and position of the C axis
 Misalignment compensation
 Single-point and double-point measurement
 Finding a hole or stud
 Zero point setting in the Z or C axis
 Automatic tool measurement
Touch probe cycles are programmed in DIN PLUS using G codes. Just
like the fixed cycles, also the touch probe cycles use transfer
parameters.
To simplify programming, the control shows a graphic during cycle
definition. The appropriate input parameters are displayed in the help
graphic (see figure at right).
The touch probe cycles save status information and measuring results
in the variable #i99. Depending on the input parameters in the touch
probe cycle you can interrogate the following values:
Result #i99
Meaning
< 999997
Measuring result
999999
Touch probe not deflected
-999999
Invalid measuring axis programmed
999998
Maximum deviation WE exceeded
999997
Maximum compensation value E exceeded
HEIDENHAIN MANUALplus 620, CNC PILOT 640
455
5.1 General information on touch probe cycles (software option)
Programming the touch probe cycle in DIN PLUS
 Select DIN PLUS programming and place the cursor in
the MACHINING program section
Beispiel: Touch probe cycle in the DINplus
program

Select "Machining" pull-down menus
HEADER

Select "G menu" pull-down menus
#MATERIAL
Steel

Select "Touch probe cycles" pull-down menus
#MEASURE_UNITS
METRIC

Select measuring cycle group

Select the cycle
TURRET 1
T1 ID"342-300.1"
Group of measuring cycles
Page
Single-point measurements
Page 457
Double-point measurements
Page 465
Calibration cycles
Page 473
Probing
Page 477
Search cycles
Page 482
Circle measurement
Page 490
N2 G0 X60 Z-115
Angle position
Page 494
N3 G1 Z-105
In-process measurement
Page 498
T2 ID"111-80-080.1"
...
BLANK
N1 G20 X120 Z120 K2
FINISHED
...
MACHINING
N19 T1
N19 G0 X0 Z5
N20 G771 R1 D0 K-30 AC0 BD2 Q0 P0 H0
N1 T2 G97 S1000 G95 F0.2 M3
N2 G0 X0 Z5
N3 G71 Z-25 A5 V2 [drilling]
...
END
456
Touch probe cycles
Single-point measurement for tool
compensation G770
Cycle G770 measures with the programmed measuring axis in the
specified direction. If the tolerance value defined in the cycle is
exceeded, the cycle saves the measured deviation either as tool
compensation or as an additive compensation. The result of the
measurement is saved additionally in the variable #i99 (See "Touch
probe cycles for automatic operation" on page 455.).
Cycle run
From the current position the touch probe moves along the defined
measuring axis toward the measuring point. When the stylus touches
the workpiece, the measured value is saved and the touch probe is
positioned back to the starting point.
The control outputs an error message if the touch probe does not
reach any touch point within the defined measuring path. If a
maximum deviation WE was programmed, the measuring point is
approached twice and the mean value is saved as result. If the
difference of the measurements is greater than the maximum
deviation WE, the program run is interrupted and an error message is
displayed.
Parameters
R
Type of compensation:
 1: Tool compensation DX/DZ for turning tool or additive
compensation
 2: Recessing tool Dx/DS
 4: Milling tool DD
D Measuring axis: Axis in which the measurement is to be made
K
Incremental measuring path with direction (signed): Maximum
measuring path for probing. The algebraic sign determines the
probing direction.
AC Nominal value for target position: Touch point coordinate
BD Tolerance +/-: Measurement result range in which no
compensation is applied
WT Compensation number T or G149:
Beispiel: G770—Single-point measurement for
tool compensation
...
MACHINING
N3 G770 R1 D0 K20 AC0 BD0.2 WT3 V1 O1 Q0
P0 H0
...
 T: Tool at turret position T to compensate the difference to the
nominal value
 G149: Additive compensation D9xx to compensate the
difference to the nominal value (only possible with
compensation type R =1)
E
Maximum compensation value for the tool compensation
WE Maximum deviation: Probe twice and monitor the dispersion of
the measured values
HEIDENHAIN MANUALplus 620, CNC PILOT 640
457
5.2 Touch probe cycles for single-point measurement
5.2 Touch probe cycles for singlepoint measurement
5.2 Touch probe cycles for single-point measurement
Parameters
V
Retraction type
O
 0: Without: Only position touch probe back to the starting
point if the touch probe was deflected
 1: Automatic: Always position touch probe back to the starting
point
Error evaluation
P
 0: Program: Do not interrupt program run, no error message
 1: Automatic: Interrupt program run and output error message
if touch probe is not deflected within measuring path
Measuring feed rate: Feed rate for probing. If nothing is entered,
the measuring feed rate from the touch probe table is used. If
the entered measuring feed rate F is higher than the one in the
touch probe table, the feed rate is reduced to the value from the
touch probe table.
Tool orientation: Orient the touch probe in the programmed
probing direction before each probing operation (machinedependent function)
PRINT outputs
H
 0: OFF: Do not display measuring results
 1: ON: Display measuring results
INPUT instead of measurement
F
Q
 0: Default: Obtain measured values by probing
 1: PC test: Simulate probing cycle on the programming station
AN Log no.: Save measurement results in
"TNC:\table\messpro.mep" table (line numbers 0–99; the table
can be expanded if necessary)
458
Touch probe cycles
Cycle G771 measures with the programmed measuring axis in the
specified direction. If the tolerance value defined in the cycle is
exceeded, the cycle saves the measured deviation as zero point shift.
The result of the measurement is saved additionally in the variable
#i99 (See "Touch probe cycles for automatic operation" on page 455.).
Cycle run
From the current position the touch probe moves along the defined
measuring axis toward the measuring point. When the stylus touches
the workpiece, the measured value is saved and the touch probe is
positioned back to the starting point.
The control outputs an error message if the touch probe does not
reach any touch point within the defined measuring path. If a
maximum deviation WE was programmed, the measuring point is
approached twice and the mean value is saved as result. If the
difference of the measurements is greater than the maximum
deviation WE, the program run is interrupted and an error message is
displayed.
Parameters
R
Type of zero point shift:
 1: Table and G59: Activate zero point shift and additionally
save in zero point table. The zero-point shift also remains
active after the program run.
 2: Activate zero point shift with G59 for the further program
run. Zero point shift no longer active after program run.
D Measuring axis: Axis in which the measurement is to be made
K
Incremental measuring path with direction (signed): Maximum
measuring path for probing. The algebraic sign determines the
probing direction.
AC Nominal value for target position: Touch point coordinate
BD Tolerance +/-: Measurement result range in which no
compensation is applied
WE Maximum deviation: Probe twice and monitor the dispersion of
the measured values
F
Measuring feed rate: Feed rate for probing. If nothing is entered,
the measuring feed rate from the touch probe table is used. If
the entered measuring feed rate F is higher than the one in the
touch probe table, the feed rate is reduced to the value from the
touch probe table.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
Beispiel: G771 Single-point measurement for tool
compensation
...
MACHINING
N3 G771 R1 D0 K20 AC0 BD0.2 Q0 P0 H0
...
459
5.2 Touch probe cycles for single-point measurement
Single-point measurement for zero point G771
5.2 Touch probe cycles for single-point measurement
Parameters
Q Tool orientation: Orient the touch probe in the programmed
probing direction before each probing operation (machinedependent function)
P
PRINT outputs
H
 0: OFF: Do not display measuring results
 1: ON: Display measuring results
INPUT instead of measurement
 0: Default: Obtain measured values by probing
 1: PC test: Simulate probing cycle on the programming station
AN Log no.: Save measurement results in
"TNC:\table\messpro.mep" table (line numbers 0–99; the table
can be expanded if necessary)
460
Touch probe cycles
Cycle G772 measures with the C axis in the specified direction. If the
tolerance value defined in the cycle is exceeded, the cycle saves the
measured deviation as zero point shift. The result of the measurement
is saved additionally in the variable #i99 (See "Touch probe cycles for
automatic operation" on page 455.).
Cycle run
From the current position, the element to be probed is moved toward
the touch probe by a rotation of the C axis. When the workpiece
touches the stylus, the measured value is saved and the workpiece is
returned.
The control outputs an error message if the touch probe does not
reach any touch point within the defined measuring path. If a
maximum deviation WE was programmed, the measuring point is
approached twice and the mean value is saved as result. If the
difference of the measurements is greater than the maximum
deviation WE, the program run is interrupted and an error message is
displayed.
Parameters
R
Type of zero point shift:
C
AC
BD
KC
WE
F
 1: Table and G152: Activate zero point shift and additionally
save in zero point table. The zero-point shift also remains
active after the program run.
 2: Activate zero point shift with G152 for the further program
run. Zero point shift no longer active after program run.
Incremental measuring path with direction: Measuring path of
the C axis (in degrees), starting from the current position. The
algebraic sign determines the probing direction.
Nominal value for target position: Absolute coordinate of touch
point in degrees
Tolerance +/-: Measurement result range (in degrees) in which
no compensation is applied
Compensation offset: Additional compensation value that is
applied to the zero point result
Maximum deviation: Probe twice and monitor the dispersion of
the measured values
Measuring feed rate: Feed rate for probing. If nothing is entered,
the measuring feed rate from the touch probe table is used. If
the entered measuring feed rate F is higher than the one in the
touch probe table, the feed rate is reduced to the value from the
touch probe table.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
Beispiel: G772—Single-point measurement zero
point C axis
...
MACHINING
N3 G772 R1 C20 AC0 BD0.2 Q0 P0 H0
...
461
5.2 Touch probe cycles for single-point measurement
Zero point C axis, single-point measurement
G772
5.2 Touch probe cycles for single-point measurement
Parameters
Q Tool orientation: Orient the touch probe in the programmed
probing direction before each probing operation (machinedependent function)
P
PRINT outputs
H
 0: OFF: Do not display measuring results
 1: ON: Display measuring results
INPUT instead of measurement
 0: Default: Obtain measured values by probing
 1: PC test: Simulate probing cycle on the programming station
AN Log no.: Save measurement results in
"TNC:\table\messpro.mep" table (line numbers 0–99; the table
can be expanded if necessary)
462
Touch probe cycles
Cycle G773 measures an element with the C axis from two opposite
sides and places the center of the element to a defined position. The
result of the measurement is saved additionally in the variable #i99
(See "Touch probe cycles for automatic operation" on page 455.).
Cycle run
From the current position, the element to be probed is moved toward
the touch probe by a rotation of the C axis. When the workpiece
touches the stylus, the measured value is saved and the workpiece is
returned. Then the touch probe is pre-positioned for the opposite
probing procedure. When the second measured value has been
determined, the cycle computes the mean value of the two
measurements and applies a zero point shift in the C axis. The nominal
position AC defined in the cycle is then in the center of the probed
element.
The control outputs an error message if the touch probe does not
reach any touch point within the defined measuring path. If a
maximum deviation WE was programmed, each measuring point is
approached twice and the mean value is saved as result. If the
difference of the measurements is greater than the maximum
deviation WE, the program run is interrupted and an error message is
displayed.
Parameters
R
Type of zero point shift:
C
E
RB
RC
AC
BD
KC
WE
F
 1: Table and G152: Activate zero point shift and additionally
save in zero point table. The zero-point shift also remains
active after the program run.
 2: Activate zero point shift with G152 for the further program
run. Zero point shift no longer active after program run.
Incremental measuring path with direction: Measuring path of
the C axis (in degrees), starting from the current position. The
algebraic sign determines the probing direction.
Circumnavigation axis: Axis that is positioned back by RB in
order to circumnavigate the element
Circumnavigation direction offset: Retraction value in the
circumnavigation axis E for pre-positioning for the next probing
position
C-angle offset: Difference in the C axis between the first and the
second measuring position
Nominal value for target position: Absolute coordinate of touch
point in degrees
Tolerance +/-: Measurement result range (in degrees) in which
no compensation is applied
Compensation offset: Additional compensation value that is
applied to the zero point result
Maximum deviation: Probe twice and monitor the dispersion of
the measured values
Measuring feed rate: Feed rate for probing. If nothing is entered,
the measuring feed rate from the touch probe table is used. If
the entered measuring feed rate F is higher than the one in the
touch probe table, the feed rate is reduced to the value from the
touch probe table.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
Beispiel: G773—Single-point measurement C-axis
object center
...
MACHINING
N3 G773 R1 C20 E0 RB20 RC45 AC30 BD0.2 Q0
P0 H0
...
463
5.2 Touch probe cycles for single-point measurement
Zero point C-axis object center G773
5.2 Touch probe cycles for single-point measurement
Parameters
Q Tool orientation: Orient the touch probe in the programmed
probing direction before each probing operation (machinedependent function)
P
PRINT outputs
H
 0: OFF: Do not display measuring results
 1: ON: Display measuring results
INPUT instead of measurement
 0: Default: Obtain measured values by probing
 1: PC test: Simulate probing cycle on the programming station
AN Log no.: Save measurement results in
"TNC:\table\messpro.mep" table (line numbers 0–99; the table
can be expanded if necessary)
464
Touch probe cycles
Two-point measurement G18 transverse G775
Cycle G775 measures two opposite points in the X/Z plane with the
measuring axis X. If the tolerance values defined in the cycle are
exceeded, the cycle saves the measured deviation either as tool
compensation or as an additive compensation. The result of the
measurement is saved additionally in the variable #i99 (See "Touch
probe cycles for automatic operation" on page 455.).
Cycle run
From the current position the touch probe moves along the defined
measuring axis toward the measuring point. When the stylus touches
the workpiece, the measured value is saved and the touch probe is
positioned back to the starting point. For the pre-positioning for the
second measurement, the cycle first moves the touch probe by the
offset in the circumnavigation direction RB and then by the offset in the
measuring direction RC. The cycle executes the second probing
operation in the opposite direction, saves the result and positions the
touch probe back with the circumnavigation axis by the
circumnavigation value.
The control outputs an error message if the touch probe does not
reach any touch point within the defined measuring path. If a
maximum deviation WE was programmed, the measuring points are
approached twice and the mean value is saved as result. If the
difference of the measurements is greater than the maximum
deviation WE, the program run is interrupted and an error message is
displayed.
Parameters
R
Type of compensation:
K
E
RB
RC
XE
BD
Beispiel: G775—Two-point measurement for tool
compensation
...
MACHINING
N3 G775 R1 K20 E1 XE30 BD0.2 X40 BE0.3
WT5 Q0 P0 H0
...
 1: Tool compensation DX/DZ for turning tool or additive
compensation
 2: Recessing tool Dx/DS
 3: Milling tool DX/DD
 4: Milling tool DD
Incremental measuring path with direction (signed): Maximum
measuring path for probing. The algebraic sign determines the
probing direction.
Circumnavigation axis: Selection of axis for retraction
movement between the probing positions:
 0: Z axis
 2: Y axis
Circumnavigation direction offset: Distance
Offset in X: Distance for pre-positioning before the second
measurement
Nominal value for target position X: Absolute coordinate of
touch point
Tolerance +/-: Range for the first measurement result in which
no compensation is applied
HEIDENHAIN MANUALplus 620, CNC PILOT 640
465
5.3 Touch probe cycles for two-point measurement
5.3 Touch probe cycles for twopoint measurement
5.3 Touch probe cycles for two-point measurement
Parameters
X
Nominal width in X: Coordinate for the second probing position
BE Tolerance width +/-: Range for the second measurement result
in which no compensation is applied
WT Compensation number T or G149, first measured edge:
 T: Tool at turret position T to compensate the difference to the
nominal value
 G149: Additive compensation D9xx to compensate the
difference to the nominal value (only possible with
compensation type R =1)
AT Compensation number T or G149, second measured edge:
 T: Tool at turret position T to compensate the difference to the
nominal value
 G149: Additive compensation D9xx to compensate the
difference to the nominal value (only possible with
compensation type R =1)
FP Maximum permissible compensation
WE Maximum deviation: Probe twice and monitor the dispersion of
the measured values
F
Measuring feed rate: Feed rate for probing. If nothing is entered,
the measuring feed rate from the touch probe table is used. If
the entered measuring feed rate F is higher than the one in the
touch probe table, the feed rate is reduced to the value from the
touch probe table.
Q Tool orientation: Orient the touch probe in the programmed
probing direction before each probing operation (machinedependent function)
P
PRINT outputs
H
 0: OFF: Do not display measuring results
 1: ON: Display measuring results
INPUT instead of measurement
 0: Default: Obtain measured values by probing
 1: PC test: Simulate probing cycle on the programming station
AN Log no.: Save measurement results in
"TNC:\table\messpro.mep" table (line numbers 0–99; the table
can be expanded if necessary)
The cycle computes the compensation value WT from the
result of the first measurement and the compensation
value AT from the result of the second measurement.
466
Touch probe cycles
Cycle G776 measures two opposite points in the X/Z plane with the
measuring axis Z. If the tolerance values defined in the cycle are
exceeded, the cycle saves the measured deviation either as tool
compensation or as an additive compensation. The result of the
measurement is saved additionally in the variable #i99 (See "Touch
probe cycles for automatic operation" on page 455.).
Cycle run
From the current position the touch probe moves along the defined
measuring axis toward the measuring point. When the stylus touches
the workpiece, the measured value is saved and the touch probe is
positioned back to the starting point. For the pre-positioning for the
second measurement, the cycle first moves the touch probe by the
offset in the circumnavigation direction RB and then by the offset in the
measuring direction RC. The cycle executes the second probing
operation in the opposite direction, saves the result and positions the
touch probe back with the circumnavigation axis by the
circumnavigation value.
The control outputs an error message if the touch probe does not
reach any touch point within the defined measuring path. If a
maximum deviation WE was programmed, the measuring points are
approached twice and the mean value is saved as result. If the
difference of the measurements is greater than the maximum
deviation WE, the program run is interrupted and an error message is
displayed.
Parameters
R
Type of compensation:
K
E
RB
RC
ZE
BD
Z
BE
Beispiel: G776—Two-point measurement for tool
compensation
...
MACHINING
N3 G776 R1 K20 E1 ZE30 BD0.2 Z40 BE0.3
WT5 Q0 P0 H0
...
 1: Tool compensation DX/DZ for turning tool or additive
compensation
 2: Recessing tool Dx/DS
 3: Milling tool DX/DD
 4: Milling tool DD
Incremental measuring path with direction (signed): Maximum
measuring path for probing. The algebraic sign determines the
probing direction.
Circumnavigation axis: Selection of axis for retraction
movement between the probing positions:
 0: X axis
 2: Y axis
Circumnavigation direction offset: Distance
Offset in Z: Distance for pre-positioning before the second
measurement
Nominal value for target position Z: Absolute coordinate of touch
point
Tolerance +/-: Range for the first measurement result in which
no compensation is applied
Nominal width in Z: Coordinate for the second probing position
Tolerance width +/-: Range for the second measurement result
in which no compensation is applied
HEIDENHAIN MANUALplus 620, CNC PILOT 640
467
5.3 Touch probe cycles for two-point measurement
Two-point measurement G18 longitudinal G776
5.3 Touch probe cycles for two-point measurement
Parameters
WT Compensation number T or G149, first measured edge:
 T: Tool at turret position T to compensate the difference to the
nominal value
 G149: Additive compensation D9xx to compensate the
difference to the nominal value (only possible with
compensation type R =1)
AT Compensation number T or G149, second measured edge:
 T: Tool at turret position T to compensate the difference to the
nominal value
 G149: Additive compensation D9xx to compensate the
difference to the nominal value (only possible with
compensation type R =1)
FP Maximum permissible compensation
WE Maximum deviation: Probe twice and monitor the dispersion of
the measured values
F
Measuring feed rate: Feed rate for probing. If nothing is entered,
the measuring feed rate from the touch probe table is used. If
the entered measuring feed rate F is higher than the one in the
touch probe table, the feed rate is reduced to the value from the
touch probe table.
Q Tool orientation: Orient the touch probe in the programmed
probing direction before each probing operation (machinedependent function)
P
PRINT outputs
H
 0: OFF: Do not display measuring results
 1: ON: Display measuring results
INPUT instead of measurement
 0: Default: Obtain measured values by probing
 1: PC test: Simulate probing cycle on the programming station
AN Log no.: Save measurement results in
"TNC:\table\messpro.mep" table (line numbers 0–99; the table
can be expanded if necessary)
The cycle computes the compensation value WT from the
result of the first measurement and the compensation
value AT from the result of the second measurement.
468
Touch probe cycles
Cycle G777 measures two opposite points in the X/Y plane with the
measuring axis Y. If the tolerance values defined in the cycle are
exceeded, the cycle saves the measured deviation either as tool
compensation or as an additive compensation. The result of the
measurement is saved additionally in the variable #i99 (See "Touch
probe cycles for automatic operation" on page 455.).
Cycle run
From the current position the touch probe moves along the defined
measuring axis toward the measuring point. When the stylus touches
the workpiece, the measured value is saved and the touch probe is
positioned back to the starting point. For the pre-positioning for the
second measurement, the cycle first moves the touch probe by the
offset in the circumnavigation direction RB and then by the offset in the
measuring direction RC. The cycle executes the second probing
operation in the opposite direction, saves the result and positions the
touch probe back with the circumnavigation axis by the
circumnavigation value.
The control outputs an error message if the touch probe does not
reach any touch point within the defined measuring path. If a
maximum deviation WE was programmed, the measuring points are
approached twice and the mean value is saved as result. If the
difference of the measurements is greater than the maximum
deviation WE, the program run is interrupted and an error message is
displayed.
Parameters
R
Type of compensation:
K
RB
RC
YE
BD
Y
BE
Beispiel: G777—Two-point measurement for tool
compensation
...
MACHINING
N3 G777 R1 K20 YE10 BD0.2 Y40 BE0.3 WT5
Q0 P0 H0
...
 1: Tool compensation DX/DZ for turning tool or additive
compensation
 2: Recessing tool Dx/DS
 3: Milling tool DX/DD
 4: Milling tool DD
Incremental measuring path with direction (signed): Maximum
measuring path for probing. The algebraic sign determines the
probing direction.
Circumnavigation direction offset: Distance in circumnavigation
direction X
Offset in Z: Distance for pre-positioning before the second
measurement
Nominal value for target position Y: Absolute coordinate of
touch point
Tolerance +/-: Range for the first measurement result in which
no compensation is applied
Nominal width in Z: Coordinate for the second probing position
Tolerance width +/-: Range for the second measurement result
in which no compensation is applied
HEIDENHAIN MANUALplus 620, CNC PILOT 640
469
5.3 Touch probe cycles for two-point measurement
Two-point measurement G17 longitudinal G777
5.3 Touch probe cycles for two-point measurement
Parameters
WT Compensation number T or G149, first measured edge:
 T: Tool at turret position T to compensate the difference to the
nominal value
 G149: Additive compensation D9xx to compensate the
difference to the nominal value (only possible with
compensation type R =1)
AT Compensation number T or G149, second measured edge:
 T: Tool at turret position T to compensate the difference to the
nominal value
 G149: Additive compensation D9xx to compensate the
difference to the nominal value (only possible with
compensation type R =1)
FP Maximum permissible compensation
WE Maximum deviation: Probe twice and monitor the dispersion of
the measured values
F
Measuring feed rate: Feed rate for probing. If nothing is entered,
the measuring feed rate from the touch probe table is used. If
the entered measuring feed rate F is higher than the one in the
touch probe table, the feed rate is reduced to the value from the
touch probe table.
Q Tool orientation: Orient the touch probe in the programmed
probing direction before each probing operation (machinedependent function)
P
PRINT outputs
H
 0: OFF: Do not display measuring results
 1: ON: Display measuring results
INPUT instead of measurement
 0: Default: Obtain measured values by probing
 1: PC test: Simulate probing cycle on the programming station
AN Log no.: Save measurement results in
"TNC:\table\messpro.mep" table (line numbers 0–99; the table
can be expanded if necessary)
The cycle computes the compensation value WT from the
result of the first measurement and the compensation
value AT from the result of the second measurement.
470
Touch probe cycles
Cycle G778 measures two opposite points in the Y/Z plane with the
measuring axis Y. If the tolerance values defined in the cycle are
exceeded, the cycle saves the measured deviation either as tool
compensation or as an additive compensation. The result of the
measurement is saved additionally in the variable #i99 (See "Touch
probe cycles for automatic operation" on page 455.).
Cycle run
From the current position the touch probe moves along the defined
measuring axis toward the measuring point. When the stylus touches
the workpiece, the measured value is saved and the touch probe is
positioned back to the starting point. For the pre-positioning for the
second measurement, the cycle first moves the touch probe by the
offset in the circumnavigation direction RB and then by the offset in the
measuring direction RC. The cycle executes the second probing
operation in the opposite direction, saves the result and positions the
touch probe back with the circumnavigation axis by the
circumnavigation value.
The control outputs an error message if the touch probe does not
reach any touch point within the defined measuring path. If a
maximum deviation WE was programmed, the measuring points are
approached twice and the mean value is saved as result. If the
difference of the measurements is greater than the maximum
deviation WE, the program run is interrupted and an error message is
displayed.
Parameters
R
Type of compensation:
K
RB
RC
ZE
BD
Z
BE
Beispiel: G778—Two-point measurement for tool
compensation
...
MACHINING
N3 G778 R1 K20 YE30 BD0.2 Y40 BE0.3 WT5
Q0 P0 H0
...
 1: Tool compensation DX/DZ for turning tool or additive
compensation
 2: Recessing tool Dx/DS
 3: Milling tool DX/DD
 4: Milling tool DD
Incremental measuring path with direction (signed): Maximum
measuring path for probing. The algebraic sign determines the
probing direction.
Circumnavigation direction offset: Distance in circumnavigation
direction X
Offset in Y: Distance for pre-positioning before the second
measurement
Nominal value for target position Y: Absolute coordinate of
touch point
Tolerance +/-: Range for the first measurement result in which
no compensation is applied
Nominal width in Y: Coordinate for the second probing position
Tolerance width +/-: Range for the second measurement result
in which no compensation is applied
HEIDENHAIN MANUALplus 620, CNC PILOT 640
471
5.3 Touch probe cycles for two-point measurement
Two-point measurement G19 longitudinal G778
5.3 Touch probe cycles for two-point measurement
Parameters
WT Compensation number T or G149, first measured edge:
 T: Tool at turret position T to compensate the difference to the
nominal value
 G149: Additive compensation D9xx to compensate the
difference to the nominal value (only possible with
compensation type R =1)
AT Compensation number T or G149, second measured edge:
 T: Tool at turret position T to compensate the difference to the
nominal value
 G149: Additive compensation D9xx to compensate the
difference to the nominal value (only possible with
compensation type R =1)
FP Maximum permissible compensation
WE Maximum deviation: Probe twice and monitor the dispersion of
the measured values
F
Measuring feed rate: Feed rate for probing. If nothing is entered,
the measuring feed rate from the touch probe table is used. If
the entered measuring feed rate F is higher than the one in the
touch probe table, the feed rate is reduced to the value from the
touch probe table.
Q Tool orientation: Orient the touch probe in the programmed
probing direction before each probing operation (machinedependent function)
P
PRINT outputs
H
 0: OFF: Do not display measuring results
 1: ON: Display measuring results
INPUT instead of measurement
 0: Default: Obtain measured values by probing
 1: PC test: Simulate probing cycle on the programming station
AN Log no.: Save measurement results in
"TNC:\table\messpro.mep" table (line numbers 0–99; the table
can be expanded if necessary)
The cycle computes the compensation value WT from the
result of the first measurement and the compensation
value AT from the result of the second measurement.
472
Touch probe cycles
5.4 Calibrating the touch probe
5.4 Calibrating the touch probe
Calibrate touch probe standard G747
Cycle G747 measures with the programmed axis and, depending on
the selected calibration method, calculates the touch probe
adjustment dimension or the ball diameter. If the tolerance values
defined in the cycle are exceeded, the cycle corrects the touch probe
data. The result of the measurement is saved additionally in the
variable #i99 (See "Touch probe cycles for automatic operation" on
page 455.).
Cycle run
From the current position the touch probe moves along the defined
measuring axis toward the measuring point. When the stylus touches
the workpiece, the measured value is saved and the touch probe is
positioned back to the starting point.
The control outputs an error message if the touch probe does not
reach any touch point within the defined measuring path. If a
maximum deviation WE was programmed, the measuring point is
approached twice and the mean value is saved as result. If the
difference of the measurements is greater than the maximum
deviation WE, the program run is interrupted and an error message is
displayed.
Parameters
R
Calibration method:
 0: Change ball diameter
 1: Change adjustment dimension
D Measuring axis: Axis in which the measurement is to be made
K
Incremental measuring path with direction (signed): Maximum
measuring path for probing. The algebraic sign determines the
probing direction.
AC Nominal value for target position: Touch point coordinate
BD Tolerance +/-: Measurement result range in which no
compensation is applied
WE Maximum deviation: Probe twice and monitor the dispersion of
the measured values
F
Measuring feed rate: Feed rate for probing. If nothing is entered,
the measuring feed rate from the touch probe table is used. If
the entered measuring feed rate F is higher than the one in the
touch probe table, the feed rate is reduced to the value from the
touch probe table.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
Beispiel: G747 Calibrate touch probe
...
MACHINING
N3 G747 R1 K20 AC10 BD0.2 Q0 P0 H0
...
473
5.4 Calibrating the touch probe
Parameters
Q Tool orientation: Orient the touch probe in the programmed
probing direction before each probing operation (machinedependent function)
P
PRINT outputs
H
 0: OFF: Do not display measuring results
 1: ON: Display measuring results
INPUT instead of measurement
 0: Default: Obtain measured values by probing
 1: PC test: Simulate probing cycle on the programming station
AN Log no.: Save measurement results in
"TNC:\table\messpro.mep" table (line numbers 0–99; the table
can be expanded if necessary)
474
Touch probe cycles
5.4 Calibrating the touch probe
Calibrate touch probe via two points G748
Cycle G748 measures two opposite points and computes the touch
probe adjustment dimension and the ball diameter. If the tolerance
values defined in the cycle are exceeded, the cycle corrects the touch
probe data. The result of the measurement is saved additionally in the
variable #i99 (See "Touch probe cycles for automatic operation" on
page 455.).
Cycle run
From the current position the touch probe moves along the defined
measuring axis toward the measuring point. When the stylus touches
the workpiece, the measured value is saved and the touch probe is
positioned back to the starting point. For the pre-positioning for the
second measurement, the cycle first moves the touch probe by the
offset in the circumnavigation direction RB and then by the offset in the
measuring direction RC. The cycle performs the second probing
operation in the opposite direction and saves the result.
The control outputs an error message if the touch probe does not
reach any touch point within the defined measuring path. If a
maximum deviation WE was programmed, the measuring points are
approached twice and the mean value is saved as result. If the
difference of the measurements is greater than the maximum
deviation WE, the program run is interrupted and an error message is
displayed.
Parameters
K
Incremental measuring path with direction (signed): Maximum
measuring path for probing. The algebraic sign determines the
probing direction.
RB Circumnavigation direction offset: Distance
RC Measuring direction offset: Distance for pre-positioning before
the second measurement
AC Nominal value for target position: Absolute coordinate of touch
point
EC Nominal width: Coordinate for the second probing position
BE Tolerance width +/-: Range for the second measurement result
in which no compensation is applied
WE Maximum deviation: Probe twice and monitor the dispersion of
the measured values
F
Measuring feed rate: Feed rate for probing. If nothing is entered,
the measuring feed rate from the touch probe table is used. If
the entered measuring feed rate F is higher than the one in the
touch probe table, the feed rate is reduced to the value from the
touch probe table.
Q Tool orientation: Orient the touch probe in the programmed
probing direction before each probing operation (machinedependent function)
P
PRINT outputs
Beispiel: G748 Calibrate touch probe via two
points
...
MACHINING
N3 G748 K20 AC10 EC33 Q0 P0 H0
...
 0: OFF: Do not display measuring results
 1: ON: Display measuring results
HEIDENHAIN MANUALplus 620, CNC PILOT 640
475
5.4 Calibrating the touch probe
Parameters
H INPUT instead of measurement
 0: Default: Obtain measured values by probing
 1: PC test: Simulate probing cycle on the programming station
AN Log no.: Save measurement results in
"TNC:\table\messpro.mep" table (line numbers 0–99; the table
can be expanded if necessary)
476
Touch probe cycles
5.5 Measuring with touch probe cycles
5.5 Measuring with touch probe
cycles
Paraxial probing G764
Cycle G764 measures with the programmed axis and displays the
measured values on the control screen. The result of the
measurement is saved additionally in the variable #i99 (See "Touch
probe cycles for automatic operation" on page 455.).
Cycle run
From the current position the touch probe moves along the defined
measuring axis toward the measuring point. When the stylus touches
the workpiece, the measured value is saved and the touch probe is
positioned back to the starting point.
The control outputs an error message if the touch probe does not
reach any touch point within the defined measuring path.
Parameters
D Measuring axis: Axis in which the measurement is to be made
K
Incremental measuring path with direction (signed): Maximum
measuring path for probing. The algebraic sign determines the
probing direction.
V
Retraction type
O
 0: Without: Only position touch probe back to the starting
point if the touch probe was deflected
 1: Automatic: Always position touch probe back to the starting
point
Error evaluation
P
 0: Program: Do not interrupt program run, no error message
 1: Automatic: Interrupt program run and output error message
if touch probe is not deflected within measuring path
Measuring feed rate: Feed rate for probing. If nothing is entered,
the measuring feed rate from the touch probe table is used. If
the entered measuring feed rate F is higher than the one in the
touch probe table, the feed rate is reduced to the value from the
touch probe table.
Tool orientation: Orient the touch probe in the programmed
probing direction before each probing operation (machinedependent function)
PRINT outputs
H
 0: OFF: Do not display measuring results
 1: ON: Display measuring results
INPUT instead of measurement
F
Q
Beispiel: G764 Paraxial probing
...
MACHINING
N3 G764 D0 K20 V1 O1 Q0 P0 H0
...
 0: Default: Obtain measured values by probing
 1: PC test: Simulate probing cycle on the programming station
HEIDENHAIN MANUALplus 620, CNC PILOT 640
477
5.5 Measuring with touch probe cycles
Probing in C axis G765
Cycle G765 measures with the C axis and displays the measured
values on the control screen. The result of the measurement is saved
additionally in the variable #i99 (See "Touch probe cycles for automatic
operation" on page 455.).
Cycle run
From the current position, the element to be probed is moved toward
the touch probe by a rotation of the C axis. When the workpiece
touches the stylus, the measured value is saved and the workpiece is
returned.
The control outputs an error message if the touch probe does not
reach any touch point within the defined measuring path.
Parameters
C
Incremental measuring path with direction: Measuring path of
the C axis (in degrees), starting from the current position. The
algebraic sign determines the probing direction.
V
Retraction type
O
 0: Without: Only position touch probe back to the starting
point if the touch probe was deflected
 1: Automatic: Always position touch probe back to the starting
point
Error evaluation
P
 0: Program: Do not interrupt program run, no error message
 1: Automatic: Interrupt program run and output error message
if touch probe is not deflected within measuring path
Measuring feed rate: Feed rate for probing. If nothing is entered,
the measuring feed rate from the touch probe table is used. If
the entered measuring feed rate F is higher than the one in the
touch probe table, the feed rate is reduced to the value from the
touch probe table.
Tool orientation: Orient the touch probe in the programmed
probing direction before each probing operation (machinedependent function)
PRINT outputs
H
 0: OFF: Do not display measuring results
 1: ON: Display measuring results
INPUT instead of measurement
F
Q
Beispiel: G765 Probing in C axis
...
MACHINING
N3 G765 C20 V1 O1 AC0 BD0.2 Q0 P0 H0
...
 0: Default: Obtain measured values by probing
 1: PC test: Simulate probing cycle on the programming station
478
Touch probe cycles
Cycle G766 measures the position programmed in the cycle in the X/
Z plane and displays the measured values on the control screen. In
parameter NF you can additionally define the variables in which the
measurement results should be saved.
Cycle run
The touch probe moves from the current position toward the
measuring point. When the stylus touches the workpiece, the
measured value is saved and the touch probe is positioned back to the
starting point.
The control outputs an error message if the touch probe does not
reach any touch point within the defined measuring path.
Parameters
Z
Target point Z: Z coordinate of measuring point
X
Target point X: X coordinate of measuring point
V
Retraction type
O
 0: Without: Only position touch probe back to the starting
point if the touch probe was deflected
 1: Automatic: Always position touch probe back to the starting
point
Error evaluation
P
 0: Program: Do not interrupt program run, no error message
 1: Automatic: Interrupt program run and output error message
if touch probe is not deflected within measuring path
Measuring feed rate: Feed rate for probing. If nothing is entered,
the measuring feed rate from the touch probe table is used. If
the entered measuring feed rate F is higher than the one in the
touch probe table, the feed rate is reduced to the value from the
touch probe table.
Tool orientation: Orient the touch probe in the programmed
probing direction before each probing operation (machinedependent function)
PRINT outputs
H
 0: OFF: Do not display measuring results
 1: ON: Display measuring results
INPUT instead of measurement
F
Q
Beispiel: G766 Probing in two axes in X/Z plane
...
MACHINING
N3 G766 Z-5 X30 V1 O1 AC0 BD0.2 Q0 P0 H0
...
 0: Default: Obtain measured values by probing
 1: PC test: Simulate probing cycle on the programming station
HEIDENHAIN MANUALplus 620, CNC PILOT 640
479
5.5 Measuring with touch probe cycles
Probing in two axes G766
5.5 Measuring with touch probe cycles
Probing in two axes G768
Cycle G768 measures the position programmed in the cycle in the Z/
Y plane and displays the measured values on the control screen. In
parameter NF you can additionally define the variables in which the
measurement results should be saved.
Cycle run
The touch probe moves from the current position toward the
measuring point. When the stylus touches the workpiece, the
measured value is saved and the touch probe is positioned back to the
starting point.
The control outputs an error message if the touch probe does not
reach any touch point within the defined measuring path.
Parameters
Z
Target point Z: Z coordinate of measuring point
Y
Target point Y: Y coordinate of measuring point
V
Retraction type
O
 0: Without: Only position touch probe back to the starting
point if the touch probe was deflected
 1: Automatic: Always position touch probe back to the starting
point
Error evaluation
 0: Program: Do not interrupt program run, no error message
 1: Automatic: Interrupt program run and output error message
if touch probe is not deflected within measuring path
F
Measuring feed rate: Feed rate for probing. If nothing is entered,
the measuring feed rate from the touch probe table is used. If
the entered measuring feed rate F is higher than the one in the
touch probe table, the feed rate is reduced to the value from the
touch probe table.
Q Tool orientation: Orient the touch probe in the programmed
probing direction before each probing operation (machinedependent function)
NF Result variable no.: Number of the first global variable in which
the result is saved (no entry = variable 810). The second
measurement result is saved automatically under the next
consecutive number.
P
PRINT outputs
H
Beispiel: G768 Probing in two axes in Z/Y plane
...
MACHINING
N3 G768 Z-5 Y10 V1 O1 AC0 BD0.2 Q0 P0 H0
...
 0: OFF: Do not display measuring results
 1: ON: Display measuring results
INPUT instead of measurement
 0: Default: Obtain measured values by probing
 1: PC test: Simulate probing cycle on the programming station
480
Touch probe cycles
Cycle G769 measures the position programmed in the cycle in the X/
Y plane and displays the measured values on the control screen. In
parameter NF you can additionally define the variables in which the
measurement results should be saved. .
Cycle run
The touch probe moves from the current position toward the
measuring point. When the stylus touches the workpiece, the
measured value is saved and the touch probe is positioned back to the
starting point.
The control outputs an error message if the touch probe does not
reach any touch point within the defined measuring path.
Parameters
X
Target point X: X coordinate of measuring point
Y
Target point Y: Y coordinate of measuring point
V
Retraction type
O
 0: Without: Only position touch probe back to the starting
point if the touch probe was deflected
 1: Automatic: Always position touch probe back to the starting
point
Error evaluation
 0: Program: Do not interrupt program run, no error message
 1: Automatic: Interrupt program run and output error message
if touch probe is not deflected within measuring path
F
Measuring feed rate: Feed rate for probing. If nothing is entered,
the measuring feed rate from the touch probe table is used. If
the entered measuring feed rate F is higher than the one in the
touch probe table, the feed rate is reduced to the value from the
touch probe table.
Q Tool orientation: Orient the touch probe in the programmed
probing direction before each probing operation (machinedependent function)
NF Result variable no.: Number of the first global variable in which
the result is saved (no entry = variable 810). The second
measurement result is saved automatically under the next
consecutive number.
P
PRINT outputs
H
Beispiel: G769 Probing in two axes in X/Y plane
...
MACHINING
N3 G769 X25 Y10 V1 O1 AC0 BD0.2 Q0 P0 H0
...
 0: OFF: Do not display measuring results
 1: ON: Display measuring results
INPUT instead of measurement
 0: Default: Obtain measured values by probing
 1: PC test: Simulate probing cycle on the programming station
HEIDENHAIN MANUALplus 620, CNC PILOT 640
481
5.5 Measuring with touch probe cycles
Probing in two axes G769
5.6 Search cycles
5.6 Search cycles
Find hole in C face G780
Cycle G780 probes the workpiece face several times with the Z axis.
Prior to each probing, the touch probe is shifted by a distance defined
in the cycle until a hole is found. Optionally, the cycle determines the
mean value by two probing operations in the hole.
If the tolerance value defined in the cycle is exceeded, the cycle saves
the measured deviation as zero point shift. The result of the
measurement is saved additionally in the variable #i99.
Result #i99
Meaning
< 999997
Result of first measurement
999999
Deviation of probing operations was higher than
programmed in Maximum Deviation parameter WE.
Cycle run
From the current position the touch probe moves along the measuring
axis Z toward the measuring point. When the stylus touches the
workpiece, the measured value is saved and the touch probe is
positioned back to the starting point. Then the cycle rotates the C axis
by the angle defined in the Search Grid parameter RC and probes again
with the Z axis. This process is repeated until a hole is found. In the
hole the cycle performs two probing operations with the C axis,
calculates the center of the hole and places the zero point in the C axis.
Beispiel: Find hole in C face G780
...
MACHINING
N3 G780 R1 D1 K2 C0 RC10 IC20 AC0 BD0.2 Q0
P0 H0
...
The control outputs an error message if the touch probe does not
reach any touch point within the defined measuring path. If a
maximum deviation WE was programmed, the measuring point is
approached twice and the mean value is saved as result. If the
difference of the measurements is greater than the maximum
deviation WE, the program run is interrupted and an error message is
displayed.
Parameters
R
Type of zero point shift:
D
K
C
482
 1: Activate table and G152 zero point shift and additionally
save in zero point table. The zero-point shift also remains
active after the program run.
 2: Activate zero point shift with G152 for the further program
run. Zero point shift no longer active after program run.
Result:
 1: Position: Set zero point without determining the hole
center. No probing operation in the hole.
 2: Object center: Before the zero point is set, determine hole
center in two probing operations with the C axis
Incremental measuring path Z (signed): Maximum measuring
path for probing. The algebraic sign determines the probing
direction.
Starting position C: Position of the C axis for the first probing
operation
Touch probe cycles
H
5.6 Search cycles
Parameters
RC Search grid Ci: Stepping angle of the C axis for the subsequent
probing operations
A
Number of points: Maximum number of probing operations
IC Measuring path in C: Measuring path of the C axis (in degrees),
starting from the current position. The algebraic sign determines
the probing direction.
AC Nominal value for target position: Absolute coordinate of touch
point in degrees
BD Tolerance +/-: Measurement result range (in degrees) in which
no compensation is applied
KC Compensation offset: Additional compensation value that is
applied to the zero point result
WE Maximum deviation: Probe twice and monitor the dispersion of
the measured values
F
Measuring feed rate: Feed rate for probing. If nothing is entered,
the measuring feed rate from the touch probe table is used. If
the entered measuring feed rate F is higher than the one in the
touch probe table, the feed rate is reduced to the value from the
touch probe table.
Q Tool orientation: Orient the touch probe in the programmed
probing direction before each probing operation (machinedependent function)
NF Result variable no.: Number of the first global variable in which
the result is saved (no entry = variable 810). The second
measurement result is saved automatically under the next
consecutive number.
P
PRINT outputs
 0: OFF: Do not display measuring results
 1: ON: Display measuring results
INPUT instead of measurement
 0: Default: Obtain measured values by probing
 1: PC test: Simulate probing cycle on the programming station
AN Log no.: Save measurement results in
"TNC:\table\messpro.mep" table (line numbers 0–99; the table
can be expanded if necessary)
HEIDENHAIN MANUALplus 620, CNC PILOT 640
483
5.6 Search cycles
Find hole in C lateral surface G781
Cycle G780 probes the lateral surface of a workpiece several times
with the X axis. Prior to each probing, the C axis is rotated by a
distance defined in the cycle until a hole is found. Optionally, the cycle
determines the mean value by two probing operations in the hole.
If the tolerance value defined in the cycle is exceeded, the cycle saves
the measured deviation as zero point shift. The result of the
measurement is saved additionally in the variable #i99.
Result #i99
Meaning
< 999997
Result of first measurement
999999
Deviation of probing operations was higher than
programmed in Maximum Deviation parameter WE.
Cycle run
From the current position the touch probe moves along the measuring
axis X toward the measuring point. When the stylus touches the
workpiece, the measured value is saved and the touch probe is
positioned back to the starting point. Then the cycle rotates the C axis
by the angle defined in the Search Grid parameter RC and probes again
with the X axis. This process is repeated until a hole is found. In the
hole the cycle performs two probing operations with the C axis,
calculates the center of the hole and sets the zero point in the C axis.
Beispiel: G781 Find hole in C face
...
MACHINING
N3 G781 R1 D1 K2 C0 RC10 IC20 AC0 BD0.2 Q0
P0 H0
...
The control outputs an error message if the touch probe does not
reach any touch point within the defined measuring path. If a
maximum deviation WE was programmed, the measuring point is
approached twice and the mean value is saved as result. If the
difference of the measurements is greater than the maximum
deviation WE, the program run is interrupted and an error message is
displayed.
Parameters
R
Type of zero point shift:
D
 1: Activate table and G152 zero point shift and additionally
save in zero point table. The zero-point shift also remains
active after the program run.
 2: Activate zero point shift with G152 for the further program
run. Zero point shift no longer active after program run.
Result:
 1: Position: Set zero point without determining the hole
center. No probing operation in the hole.
 2: Object center: Before the zero point is set, determine hole
center in two probing operations with the C axis
K
Incremental measuring path X (signed): Maximum measuring
path for probing. The algebraic sign determines the probing
direction.
C
Starting position C: Position of the C axis for the first probing
operation
RC Search grid Ci: Stepping angle of the C axis for the subsequent
probing operations
A
Number of points: Maximum number of probing operations
484
Touch probe cycles
H
5.6 Search cycles
Parameters
IC Measuring path in C: Measuring path of the C axis (in degrees),
starting from the current position. The algebraic sign determines
the probing direction.
AC Nominal value for target position: Absolute coordinate of touch
point in degrees
BD Tolerance +/-: Measurement result range (in degrees) in which
no compensation is applied
KC Compensation offset: Additional compensation value that is
applied to the zero point result
WE Maximum deviation: Probe twice and monitor the dispersion of
the measured values
F
Measuring feed rate: Feed rate for probing. If nothing is entered,
the measuring feed rate from the touch probe table is used. If
the entered measuring feed rate F is higher than the one in the
touch probe table, the feed rate is reduced to the value from the
touch probe table.
Q Tool orientation: Orient the touch probe in the programmed
probing direction before each probing operation (machinedependent function)
P
PRINT outputs
 0: OFF: Do not display measuring results
 1: ON: Display measuring results
INPUT instead of measurement
 0: Default: Obtain measured values by probing
 1: PC test: Simulate probing cycle on the programming station
AN Log no.: Save measurement results in
"TNC:\table\messpro.mep" table (line numbers 0–99; the table
can be expanded if necessary)
HEIDENHAIN MANUALplus 620, CNC PILOT 640
485
5.6 Search cycles
Find stud in C face G782
Cycle G782 probes the workpiece face several times with the Z axis.
Prior to each probing, the C axis is rotated by a distance defined in the
cycle until a stud is found. Optionally, the cycle determines the mean
value by two probing operations on the stud diameter.
If the tolerance value defined in the cycle is exceeded, the cycle saves
the measured deviation as zero point shift. The result of the
measurement is saved additionally in the variable #i99.
Result #i99
Meaning
< 999997
Result of first measurement
999999
Deviation of probing operations was higher than
programmed in Maximum Deviation parameter WE.
Cycle run
From the current position the touch probe moves along the measuring
axis X toward the measuring point. When the stylus touches the
workpiece, the measured value is saved and the touch probe is
positioned back to the starting point. Then the cycle rotates the C axis
by the angle defined in the Search Grid parameter RC and probes again
with the X axis. This process is repeated until a stud is found. The
cycle performs two probing operations on the stud diameter with the
C axis, calculates the center of the hole and sets the zero point in the
C axis.
Beispiel: G782 Find stud in C face
...
MACHINING
N3 G782 R1 D1 K2 C0 RC10 IC20 AC0 BD0.2 Q0
P0 H0
...
The control outputs an error message if the touch probe does not
reach any touch point within the defined measuring path. If a
maximum deviation WE was programmed, the measuring point is
approached twice and the mean value is saved as result. If the
difference of the measurements is greater than the maximum
deviation WE, the program run is interrupted and an error message is
displayed.
Parameters
R
Type of zero point shift:
D
 1: Activate table and G152 zero point shift and additionally
save in zero point table. The zero-point shift also remains
active after the program run.
 2: Activate zero point shift with G152 for the further program
run. Zero point shift no longer active after program run.
Result:
 1: Position: Set zero point without determining the stud
center. The stud diameter is not probed.
 2: Object center: Before the zero point is set, determine stud
center in two probing operations with the C axis
K
Incremental measuring path X (signed): Maximum measuring
path for probing. The algebraic sign determines the probing
direction.
C
Starting position C: Position of the C axis for the first probing
operation
RC Search grid Ci: Stepping angle of the C axis for the subsequent
probing operations
486
Touch probe cycles
H
5.6 Search cycles
Parameters
A
Number of points: Maximum number of probing operations
IC Measuring path in C: Measuring path of the C axis (in degrees),
starting from the current position. The algebraic sign determines
the probing direction.
AC Nominal value for target position: Absolute coordinate of touch
point in degrees
BD Tolerance +/-: Measurement result range (in degrees) in which
no compensation is applied
KC Compensation offset: Additional compensation value that is
applied to the zero point result
WE Maximum deviation: Probe twice and monitor the dispersion of
the measured values
F
Measuring feed rate: Feed rate for probing. If nothing is entered,
the measuring feed rate from the touch probe table is used. If
the entered measuring feed rate F is higher than the one in the
touch probe table, the feed rate is reduced to the value from the
touch probe table.
Q Tool orientation: Orient the touch probe in the programmed
probing direction before each probing operation (machinedependent function)
P
PRINT outputs
 0: OFF: Do not display measuring results
 1: ON: Display measuring results
INPUT instead of measurement
 0: Default: Obtain measured values by probing
 1: PC test: Simulate probing cycle on the programming station
AN Log no.: Save measurement results in
"TNC:\table\messpro.mep" table (line numbers 0–99; the table
can be expanded if necessary)
HEIDENHAIN MANUALplus 620, CNC PILOT 640
487
5.6 Search cycles
Find stud in C lateral surface G783
Cycle G783 probes the workpiece face several times with the X axis.
Prior to each probing, the touch probe is shifted by a distance defined
in the cycle until a stud is found. Optionally, the cycle determines the
mean value by two probing operations on the stud diameter.
If the tolerance value defined in the cycle is exceeded, the cycle saves
the measured deviation as zero point shift. The result of the
measurement is saved additionally in the variable #i99.
Result #i99
Meaning
< 999997
Result of first measurement
999999
Deviation of probing operations was higher than
programmed in Maximum Deviation parameter WE.
Cycle run
From the current position the touch probe moves along the measuring
axis Z toward the measuring point. When the stylus touches the
workpiece, the measured value is saved and the touch probe is
positioned back to the starting point. Then the cycle rotates the C axis
by the angle defined in the Search Grid parameter RC and probes again
with the Z axis. This process is repeated until a stud is found. The cycle
performs two probing operations on the stud diameter with the C axis,
calculates the center of the hole and sets the zero point in the C axis.
Beispiel: G783 Find stud in C lateral surface
...
MACHINING
N3 G783 R1 D1 K2 C0 RC10 IC20 AC0 BD0.2 Q0
P0 H0
...
The control outputs an error message if the touch probe does not
reach any touch point within the defined measuring path. If a
maximum deviation WE was programmed, the measuring point is
approached twice and the mean value is saved as result. If the
difference of the measurements is greater than the maximum
deviation WE, the program run is interrupted and an error message is
displayed.
Parameters
R
Type of zero point shift:
D
 1: Activate table and G152 zero point shift and additionally
save in zero point table. The zero-point shift also remains
active after the program run.
 2: Activate zero point shift with G152 for the further program
run. Zero point shift no longer active after program run.
Result:
 1: Position: Set zero point without determining the stud
center. The stud diameter is not probed.
 2: Object center: Before the zero point is set, determine stud
center in two probing operations with the C axis
K
Incremental measuring path Z (signed): Maximum measuring
path for probing. The algebraic sign determines the probing
direction.
C
Starting position C: Position of the C axis for the first probing
operation
RC Search grid Ci: Stepping angle of the C axis for the subsequent
probing operations
A
Number of points: Maximum number of probing operations
488
Touch probe cycles
H
5.6 Search cycles
Parameters
IC Measuring path in C: Measuring path of the C axis (in degrees),
starting from the current position. The algebraic sign determines
the probing direction.
AC Nominal value for target position: Absolute coordinate of touch
point in degrees
BD Tolerance +/-: Measurement result range (in degrees) in which
no compensation is applied
KC Compensation offset: Additional compensation value that is
applied to the zero point result
WE Maximum deviation: Probe twice and monitor the dispersion of
the measured values
F
Measuring feed rate: Feed rate for probing. If nothing is entered,
the measuring feed rate from the touch probe table is used. If
the entered measuring feed rate F is higher than the one in the
touch probe table, the feed rate is reduced to the value from the
touch probe table.
Q Tool orientation: Orient the touch probe in the programmed
probing direction before each probing operation (machinedependent function)
P
PRINT outputs
 0: OFF: Do not display measuring results
 1: ON: Display measuring results
INPUT instead of measurement
 0: Default: Obtain measured values by probing
 1: PC test: Simulate probing cycle on the programming station
AN Log no.: Save measurement results in
"TNC:\table\messpro.mep" table (line numbers 0–99; the table
can be expanded if necessary)
HEIDENHAIN MANUALplus 620, CNC PILOT 640
489
5.7 Circular measurement
5.7 Circular measurement
Circular measurement G785
Cycle G785 determines the circle center and diameter by probing
three times in the programmed plane and shows the measured values
on the control screen. The result of the measurement is saved
additionally in the variable #i99 (See "Touch probe cycles for automatic
operation" on page 455.).
Cycle run
From the current position the touch probe moves in the defined
measuring plane toward the measuring point. When the stylus
touches the workpiece, the measured value is saved and the touch
probe is positioned back to the starting point. Another two probing
operations are carried out with the defined stepping angle. If a starting
diameter D was programmed, the cycle positions the touch probe on
a circular path before the respective measuring process.
The control outputs an error message if the touch probe does not
reach any touch point within the defined measuring path. If a
maximum deviation WE was programmed, the measuring point is
approached twice and the mean value is saved as result. If the
difference of the measurements is greater than the maximum
deviation WE, the program run is interrupted and an error message is
displayed.
Parameters
R
Type of zero point shift:
Beispiel: G785 Circular measurement
...
MACHINING
N3 G785 R0 BR0 K2 C0 RC60 I0 J0 Q0 P0 H0
...
 0: X/Y plane G17: Probe circle in X/Y plane
 1: Z/X plane G18: Probe circle in Z/X plane
 2: Y/Z plane G19: Probe circle in Y/Z plane
BR Inside/outside:
 0: Inside: Probe inside diameter
 1: Outside: Probe outside diameter
K
Incremental measuring path (signed): Maximum measuring path
for probing. The algebraic sign determines the probing direction.
C
Angle of 1st measurement: Angle for the first probing operation
RC Incremental angle: Stepping angle for the subsequent probing
operations
D Starting diameter: Diameter on which the touch probe is prepositioned before the measurements.
WB Position in infeed direction: Measuring height to which the
touch probe is positioned before the measuring process. No
input: The circle is probed from the current position.
I
Circle center in axis 1: Nominal position of the circle center in
first axis
J
Circle center in axis 2: Nominal position of the circle center in
second axis
WE Maximum deviation: Probe twice and monitor the dispersion of
the measured values
490
Touch probe cycles
H
5.7 Circular measurement
Parameters
F
Measuring feed rate: Feed rate for probing. If nothing is entered,
the measuring feed rate from the touch probe table is used. If
the entered measuring feed rate F is higher than the one in the
touch probe table, the feed rate is reduced to the value from the
touch probe table.
Q Tool orientation: Orient the touch probe in the programmed
probing direction before each probing operation (machinedependent function)
NF Result variable no.: Number of the first global variable in which
the result is saved (no entry = variable 810). The second
measurement result is saved automatically under the next
consecutive number.
P
PRINT outputs
 0: OFF: Do not display measuring results
 1: ON: Display measuring results
INPUT instead of measurement
 0: Default: Obtain measured values by probing
 1: PC test: Simulate probing cycle on the programming station
AN Log no.: Save measurement results in
"TNC:\table\messpro.mep" table (line numbers 0–99; the table
can be expanded if necessary)
HEIDENHAIN MANUALplus 620, CNC PILOT 640
491
5.7 Circular measurement
Determine pitch circle G786
Cycle G786 determines the center and diameter of a pitch circle by
measuring three holes and shows the measured values on the control
screen. The result of the measurement is saved additionally in the
variable #i99 (See "Touch probe cycles for automatic operation" on
page 455.).
Cycle run
From the current position the touch probe moves in the defined
measuring plane toward the measuring point. When the stylus
touches the workpiece, the measured value is saved and the touch
probe is positioned back to the starting point. Another two probing
operations are carried out with the defined stepping angle. If a starting
diameter D was programmed, the cycle positions the touch probe on
a circular path before the respective measuring process.
The control outputs an error message if the touch probe does not
reach any touch point within the defined measuring path. If a
maximum deviation WE was programmed, the measuring point is
approached twice and the mean value is saved as result. If the
difference of the measurements is greater than the maximum
deviation WE, the program run is interrupted and an error message is
displayed.
Parameters
R
Type of zero point shift:
K
C
AC
RC
WB
I
J
D
WS
WC
BD
BE
WE
492
 0: X/Y plane G17: Probe circle in X/Y plane
 1: Z/X plane G18: Probe circle in Z/X plane
 2: Y/Z plane G19: Probe circle in Y/Z plane
Incremental measuring path: Maximum measuring path for
measurement in the holes.
Angle of 1st hole: Angle for the first probing operation
Angle of 2nd hole: Angle for the second probing operation
Angle of 3rd hole: Angle for the third probing operation
Position in infeed direction: Measuring height to which the
touch probe is positioned before the measuring process. No
input: The hole is probed from the current position.
Pitch circle center in axis 1: Nominal position of the pitch circle
center in first axis
Pitch circle center in axis 2: Nominal position of the pitch circle
center in second axis
Nominal diameter: Diameter on which the touch probe is prepositioned before the measurements.
Max. diameter of pitch circle
Min. diameter of pitch circle
Tolerance for center in first axis
Tolerance for center in second axis
Maximum deviation: Probe twice and monitor the dispersion of
the measured values
Beispiel: G786 Determine pitch circle
...
MACHINING
N3 G786 R0 K8 I0 J0 D50 WS50.1 WC49.9
BD0.1 BE0.1 P0 H0
...
Touch probe cycles
H
5.7 Circular measurement
Parameters
F
Measuring feed rate: Feed rate for probing. If nothing is entered,
the measuring feed rate from the touch probe table is used. If
the entered measuring feed rate F is higher than the one in the
touch probe table, the feed rate is reduced to the value from the
touch probe table.
Q Tool orientation: Orient the touch probe in the programmed
probing direction before each probing operation (machinedependent function)
NF Result variable no.: Number of the first global variable in which
the result is saved (no entry = variable 810). The second
measurement result is saved automatically under the next
consecutive number.
P
PRINT outputs
 0: OFF: Do not display measuring results
 1: ON: Display measuring results
INPUT instead of measurement
 0: Default: Obtain measured values by probing
 1: PC test: Simulate probing cycle on the programming station
AN Log no.: Save measurement results in
"TNC:\table\messpro.mep" table (line numbers 0–99; the table
can be expanded if necessary)
HEIDENHAIN MANUALplus 620, CNC PILOT 640
493
5.8 Angular measurement
5.8 Angular measurement
Angular measurement G787
Cycle G787 probes twice in the programmed direction and computes
the angle. If the tolerance value defined in the cycle is exceeded, the
cycle saves the measured deviation for a subsequent misalignment
compensation. Program Cycle G788 next in order to activate the
misalignment compensation. The result of the measurement is saved
additionally in the variable #i99 (See "Touch probe cycles for automatic
operation" on page 455.).
Cycle run
From the current position the touch probe moves along the defined
measuring axis toward the measuring point. When the stylus touches
the workpiece, the measured value is saved and the touch probe is
retracted. Then the touch probe is pre-positioned for the second
measurement and the workpiece is probed.
The control outputs an error message if the touch probe does not
reach any touch point within the defined measuring path. If a
maximum deviation WE was programmed, the measuring point is
approached twice and the mean value is saved as result. If the
difference of the measurements is greater than the maximum
deviation WE, the program run is interrupted and an error message is
displayed.
Parameters
R
Evaluation:
D
K
WS
WC
AC
BE
RC
BD
494
 1: Prepare tool compensation and misalignment
compensation:
 2: Prepare misalignment compensation:
 3: Angle output:
Directions:
Beispiel: G787 Angular measurement
...
MACHINING
N3 G787 R1 D0 BR0 K2 WS-2 WC15 AC170 BE1
RC0 BD0.2 WT3 Q0 P0 H0
...
 0: X measurement, Z offset
 1: Y measurement, Z offset
 2: Z measurement, X offset
 3: Y measurement, X offset
 4: Z measurement, Y offset
 5: X measurement, Y offset
Incremental measuring path (signed): Maximum measuring path
for probing. The algebraic sign determines the probing direction.
Position of first measuring point
Position of second measuring point
Nominal angle of measured surface
Angle tolerance +/-: Measurement result range (in degrees) in
which no compensation is applied
Target position of first measurement: Nominal value of first
measuring point
Tolerance of first measurement +/-: Measurement result range
in which no compensation is applied
Touch probe cycles
5.8 Angular measurement
Parameters
WT Compensation number T or G149, first measured edge:
 T: Tool at turret position T to compensate the difference to the
nominal value
 G149: Additive compensation D9xx to compensate the
difference to the nominal value (only possible with
compensation type R =1)
FP Maximum permissible compensation
WE Maximum deviation: Probe twice and monitor the dispersion of
the measured values
F
Measuring feed rate: Feed rate for probing. If nothing is entered,
the measuring feed rate from the touch probe table is used. If
the entered measuring feed rate F is higher than the one in the
touch probe table, the feed rate is reduced to the value from the
touch probe table.
Q Tool orientation: Orient the touch probe in the programmed
probing direction before each probing operation (machinedependent function)
NF Result variable no.: Number of the first global variable in which
the result is saved (no entry = variable 810). The second
measurement result is saved automatically under the next
consecutive number.
P
PRINT outputs
H
 0: OFF: Do not display measuring results
 1: ON: Display measuring results
INPUT instead of measurement
 0: Default: Obtain measured values by probing
 1: PC test: Simulate probing cycle on the programming station
AN Log no.: Save measurement results in
"TNC:\table\messpro.mep" table (line numbers 0–99; the table
can be expanded if necessary)
HEIDENHAIN MANUALplus 620, CNC PILOT 640
495
5.8 Angular measurement
Misalignment compensation after angle
measurement G788
Cycle G788 activates a misalignment compensation determined with
Cycle G787 Angle Measurement.
Parameters
NF Result variable no.: Number of the first global variable in which
the result is saved (no entry = variable 810). The second
measurement result is saved automatically under the next
consecutive number.
P
Compensation
 0: OFF: Do not perform misalignment compensation
 1: ON: Perform misalignment compensation
Beispiel: G788 Misalignment compensation after
angle measurement
...
MACHINING
N3 G788 NF1 P0
...
496
Touch probe cycles
5.9 In-process measurement
5.9 In-process measurement
Measure workpieces (option)
In-process measurement is measurement at the workpiece with a
touch probe located in a tool holder of the machine. In the tool list,
enter your touch probe as a new tool. Use the tool type "length gauge."
The following cycles for "in-process measurement" are basic cycles for
probing functions that you can use to program individually adapted
probing sequences.
Switch on measurement G910
G910 activates the selected touch probe.
Parameters
H
Measuring direction (no function)
V
Type of measurement
 0: Touch probe (for workpiece measurement)
 1: Table-mounted touch probe (for tool measurement)
Beispiel: In-process measurement
...
N1 G0 X105 Z-20
N2 G94 F500
N3 G910 H0 V0
N4 G911 V0
N4 G1 Xi-10
N5 G914
N4 G912 Q1
N4 G913
N4 G0 X115
N4 #l1=#a9(X,0)
N4 IF NDEF(#l1)
N4 THEN
N4
PRINT("Probe not reached")
N4 ELSE
N4
PRINT ("Result of measurement:",#l1)
N4 ENDIF
...
HEIDENHAIN MANUALplus 620, CNC PILOT 640
497
5.9 In-process measurement
Measuring path monitoring G911
G911 activates the measuring path monitoring. Then only a single feed
path is permissible.
Parameters
V
 0: Axes stay stationary with deflected touch probe
 1: Axes automatically retract after deflection of the touch
probe
Measured value capture G912
G912 puts the positions at which the touch probe was deflected into
the result variables.
Parameters
Q
Error evaluation when the touch probe is not reached
 0: Error message of NC, program stops
 1: Error evaluation in the NC program, measuring
results="NDEF"
The measurement results are available in the following
variables:
Beispiel: Measurement results:
...
N1 #l1=#a9(X,0) [X value of current channel]
N2 #l2=#a9(Z,1) [Z value of channel 1 ]
N3 #l3=#a9(Y,0) [Y value of current channel]
N4 #l4=#a9(C,0) [C value of current channel]
...
#a9(axis,channel)
Axis=axis name
Channel=channel number, 0=current channel
End in-process measuring G913
G913 ends the measuring process.
Switch off measuring-path monitoring G914
G914 deactivates the measuring-path monitoring.
498
Touch probe cycles
5.9 In-process measurement
In-process measurement example: Measuring
and compensating workpieces
The Steuerung provides subprograms for the measurement of
workpieces:
 measure_pos.ncs
 measure_pos_e.ncs
(German dialog texts)
(English dialog texts)
The programs require a touch probe as a tool. Beginning from the
current position or the defined starting position, the Steuerung moves
along a measuring path in the entered axis direction. At the end it
returns again to the previous position. The result of measurement can
be included in error compensation.
The following subprograms are used:
 measure_pos_move.ncs
 _Print_txt_lang.ncs
Parameters
LA
Measurement starting point in X (diameter value)—no input,
current position.
LB
Measurement starting point in Z (no input = current
position).
LC
Type of approach to measurement starting point
LD
 0: Diagonal
 1: First X, then Z
 2: First Z, then X
Measuring axis
LJ
LK
 0: X axis
 1: Z axis
 2: Y axis
Incremental measurement path. The algebraic sign defines
the direction of traverse.
Measuring feed rate in mm/min—no input, the measuring
feed rate from the touch probe table is used.
Nominal value of the target position
Tolerance +/-. If the measured deviation lies within this
tolerance, the entered compensation value is not changed.
1: The measurement result is output as PRINT.
Number of the compensation value to be changed.
LO
 1-xx Turret pocket number of the tool to be compensated
 901-916 Additive compensation
 Current tool number for touch probe calibration
Number of measurements:
LE
LF
LH
LI
 >0: The measurements are evenly distributed on the
circumference with M19.
 <0: The measurements are made at the same position.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
499
5.9 In-process measurement
Parameters
LP
Maximum permissible difference between the
measurement results at a position. The program stops if the
limit is violated.
LR
Maximum permissible compensation value, <10 mm
LS
1: Program runs on the PC. Measurement results are
interrogated through INPUT. For test purposes.
In-process measurement example: Measuring
and compensating workpieces
(measure_pos_move.ncs)
For the program "measure_pos_move.ncs" you have to use a touch
probe as tool. The control moves the touch probe from the actual
position in the given axis direction. After reaching the contact position,
it returns again to the previous position. The measurement result can
then be used again.
Parameters
LA
Measuring axis:
LC
LD
 0: X axis
 1: Z axis
 2: Y axis
 3: C axis
Incremental measurement path. The algebraic sign defines
the direction of traverse.
Measuring feed rate in mm/min
Retraction type
LO
 0: Return with G0 to starting point
 1: Return automatically to starting point
Error response from missing stylus deflection:
LB
LF
LS
500
 0: A PRINT output follows and the program does not stop.
A further response in the program is possible.
 1: The program stops with an NC error message.
1: The measurement result is output as PRINT.
1: Program runs on the PC. Measurement results are
interrogated through INPUT. For test purposes.
Touch probe cycles
DIN programming
for the Y axis
HEIDENHAIN MANUALplus 620, CNC PILOT 640
501
6.1 Y-axis contours—Fundamentals
6.1 Y-axis contours—
Fundamentals
Position of milling contours
Define the reference plane or the reference diameter in the section
code. Specify the depth and position of a milling contour (pocket,
island) in the contour definition:
 With depth P programmed in the previous G308 cycle
 Alternatively on figures: Cycle parameter depth P
The algebraic sign of "P" defines the position of the milling contour:
 P<0: Pocket
 P>0: Island
Position of milling contour
Section
P
Surface
Milling floor
FACE
P<0
Z
Z+P
P>0
Z+P
Z
P<0
Z
Z–P
P>0
Z–P
Z
P<0
X
X+(P*2)
P>0
X+(P*2)
X
REAR
LATERAL
 X: Reference diameter from the section code
 Z: Reference plane from the section code
 P: Depth from G308 or from the figure definition
The area milling cycles mill the surface specified in the
contour definition. Islands within this surface are not
taken into consideration.
502
DIN programming for the Y axis
6.1 Y-axis contours—Fundamentals
Cutting limit
If parts of the milling contour lie outside of the turning contour, you
must limit the machining area with the area diameter X / reference
diameter X (parameters of the section code or of the figure
definition).
HEIDENHAIN MANUALplus 620, CNC PILOT 640
503
6.2 Contours in the XY plane
6.2 Contours in the XY plane
Starting point of contour in XY plane G170-Geo
G170 defines the starting point of a contour in the XY plane.
Parameters
X
Starting point of contour (radius)
Y
Starting point of contour
PZ
Starting point (polar radius)
W
Starting point (polar angle)
Line segment in XY plane G171-Geo
G171 defines a line segment in a contour of the XY plane.
Parameters
X
End point (radius)
Y
End point
AN Angle to X axis (for direction of angle, see help graphic)
Q
Point of intersection. End point if the line segment intersects a
circular arc (default: 0):
BR
PZ
W
AR
R
 0: Near point of intersection
 1: Far point of intersection
Chamfer/rounding. Defines the transition to the next contour
element. When entering a chamfer/rounding, program the
theoretical end point.
 No entry: Tangential transition
 BR=0: No tangential transition
 BR>0: Radius of rounding
 BR<0: Width of chamfer
End point (polar radius; reference: workpiece zero point)
End point (polar angle; reference: workpiece zero point)
Angle (AR corresponds to AN)
Length (polar radius; reference: last contour point)
Programming
 X, Y: Absolute, incremental, modal or "?"
 ANi: Angle to the subsequent element
 ARi: Angle to the previous element
504
DIN programming for the Y axis
6.2 Contours in the XY plane
Circular arc in XY plane G172-Geo/G173-Geo
G172/G173 defines a circular arc in a contour of the XY plane. Direction
of rotation: See help graphic
Parameters
X
End point (radius)
Y
End point
R
Radius
I
Center in X direction (radius)
J
Center in Y direction
Q
Point of intersection. End point if the circular arc intersects a
line segment or another circular arc (default: 0):
BR
 0: Near point of intersection
 1: Far point of intersection
Chamfer/rounding. Defines the transition to the next contour
element. When entering a chamfer/rounding, program the
theoretical end point.
 No entry: Tangential transition
 BR=0: No tangential transition
 BR>0: Radius of rounding
 BR<0: Width of chamfer
PZ
End point (polar radius; reference: workpiece zero point)
W
End point (polar angle; reference: workpiece zero point)
PM Center point (polar radius; reference: workpiece zero point)
WM Center point (polar angle; reference: workpiece zero point)
AR Starting angle (tangential angle to rotary axis)
AN End angle (tangential angle to rotary axis)
Programming
 X, Y: Absolute, incremental, modal or "?"
 I, J: Absolute or incremental
 PZ, W, PM, WM: Absolute or incremental
 ARi: Angle to the previous element
 ANi: Angle to the subsequent element
 End point must not be the starting point (no full circle).
HEIDENHAIN MANUALplus 620, CNC PILOT 640
505
6.2 Contours in the XY plane
Hole in XY plane G370-Geo
G370 defines a hole with countersinking and thread in the XY plane.
Parameters
X
Center of hole (radius)
Y
Center of hole
B
Hole diameter
P
Depth of hole (excluding point)
W
Point angle (default: 180°)
R
Sinking diameter
U
Sinking depth
E
Sinking angle
I
Thread diameter
J
Thread depth
K
Start of thread (runout length)
F
Thread pitch
V
Left-hand or right-hand thread (default: 0)
A
 0: Right-hand thread
 1: Left-hand thread
Angle to Z axis. Inclination of the hole
O
 Front face (range: –90° < A < 90°; default: 0°)
 Rear face (range: 90° < A < 270°; default: 180°)
Centering diameter
506
DIN programming for the Y axis
6.2 Contours in the XY plane
Linear slot in XY plane G371-Geo
G371 defines the contour of a linear slot in the XY plane.
Parameters
X
Center of slot (radius)
Y
Center of slot
K
Slot length
B
Slot width
A
Position angle (reference: positive X axis; default: 0°)
P
Depth/height (default: "P" from G308)
I
 P<0: Pocket
 P>0: Island
Limit diameter (as cutting limit)
 No input: "X" from section code
 "I" overwrites "X" from section code
HEIDENHAIN MANUALplus 620, CNC PILOT 640
507
6.2 Contours in the XY plane
Circular slot in XY plane G372-Geo/G373-Geo
G372/G373 defines a circular slot in the XY plane.
 G372: Circular slot clockwise
 G373: Circular slot counterclockwise
Parameters
X
Center of slot curvature (radius)
Y
Center of slot curvature
R
Curvature radius (reference: center point path of the slot)
A
Starting angle (reference: positive X axis; default: 0°)
W
End angle (reference: positive X axis; default: 0°)
B
Slot width
P
Depth/height (default: "P" from G308)
I
 P<0: Pocket
 P>0: Island
Limit diameter (as cutting limit)
 No input: "X" from section code
 "I" overwrites "X" from section code
Full circle in XY plane G374-Geo
G374 defines a full circle in the XY plane.
Parameters
X
Circle center (radius)
Y
Circle center
R
Circle radius
P
Depth/height (default: "P" from G308)
I
 P<0: Pocket
 P>0: Island
Limit diameter (as cutting limit)
 No input: "X" from section code
 "I" overwrites "X" from section code
508
DIN programming for the Y axis
6.2 Contours in the XY plane
Rectangle in XY plane G375-Geo
G375 defines a rectangle in the XY plane.
Parameters
X
Center of rectangle (radius)
Y
Center of rectangle
A
Position angle (reference: positive X axis; default: 0°)
K
Length of rectangle
B
Width of rectangle
R
Chamfer/rounding (default: 0)
P
 R>0: Radius of rounding
 R<0: Width of chamfer
Depth/height (default: "P" from G308)
I
 P<0: Pocket
 P>0: Island
Limit diameter (as cutting limit)
 No input: "X" from section code
 "I" overwrites "X" from section code
Eccentric polygon in XY plane G377-Geo
G377 defines the contour of an eccentric polygon in the XY plane.
Parameters
X
Center point of polygon (radius)
Y
Center point of polygon
Q
Number of corners (Q >= 3)
A
Position angle (reference: positive X axis; default: 0°)
K
Edge length / width across flats
R
 K>0: Edge length
 K<0: Width across flats (inside diameter)
Chamfer/rounding—default: 0
P
 R>0: Radius of rounding
 R<0: Width of chamfer
Depth/height (default: "P" from G308)
I
 P<0: Pocket
 P>0: Island
Limit diameter (as cutting limit)
 No input: "X" from section code
 "I" overwrites "X" from section code
HEIDENHAIN MANUALplus 620, CNC PILOT 640
509
6.2 Contours in the XY plane
Linear pattern in XY plane G471-Geo
G471 defines a linear pattern in the XY plane. G471 is effective for the
hole or figure defined in the following block (G370 to G375, G377).
Parameters
Q
Number of figures
X
1st point of pattern (radius)
Y
1st point of pattern
I
End point of pattern (X direction; radius)
J
End point of pattern (Y direction)
Ii
Distance in X direction between two figures
Ji
Distance in Y direction between two figures
A
Position angle of longitudinal axis of pattern (reference:
positive X axis)
R
Length (overall length of pattern)
Ri
Pattern distance (distance between two figures)
Programming notes
 Program the hole/figure in the following block without a
center.
 The milling cycle (MACHINING section) calls the hole/
figure in the following block—not the pattern definition.
510
DIN programming for the Y axis
6.2 Contours in the XY plane
Circular pattern in XY plane G472-Geo
G472 defines a circular pattern in the XY plane. G472 is effective for
the figure defined in the following block (G370 to G375, G377).
Parameters
Q
Number of figures
K
Diameter (pattern diameter)
A
Starting angle—position of the first figure (reference: positive
X axis; default: 0°)
W
End angle—position of the last figure (reference: positive X
axis; default: 360°)
Wi
Angle between two figures
V
Direction—orientation (default: 0)
X
Y
H
 V=0, without W: Figures are arranged on a full circle
 V=0, with W: Figures are arranged on the longer circular arc
 V=0, with Wi: The algebraic sign of Wi defines the direction
(Wi<0: clockwise)
 V=1, with W: Clockwise
 V=1, with Wi: Clockwise (algebraic sign of Wi has no effect)
 V=2, with W: Counterclockwise
 V=2, with Wi: Counterclockwise (algebraic sign of Wi has no
effect)
Center of pattern (radius)
Center of pattern
Position of the figures (default: 0)
 0: Normal position—the figures are rotated about the circle
center (rotation)
 1: Original position—the position of the figures relative to the
coordinate system remains unchanged (translation)
 Program the hole/figure in the following block without a
center. Exception: circular slot.
 The milling cycle (MACHINING section) calls the hole/
figure in the following block—not the pattern definition.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
511
6.2 Contours in the XY plane
Single surface in XY plane G376-Geo
G376 defines a surface in the XY plane.
Parameters
Z
Reference edge (default: "Z" from section code)
K
Residual depth
Ki
Depth
B
Width (reference: reference edge Z)
I
 B<0: Surface in negative Z direction
 B>0: Surface in positive Z direction
Limit diameter (as cutting limit and as reference for K/Ki)
C
 No input: "X" from section code
 "I" overwrites "X" from section code
Spindle angle of surface normal (default: "C" from section code)
Whether the surface lies on the front face or rear side has
no effect on the evaluation of the algebraic sign for "width
B."
Centric polygon in XY plane G477-Geo
G477 defines polygonal surfaces in the XY plane.
Parameters
Z
Reference edge (default: "Z" from section code)
K
Width across flats (inscribed circle diameter)
Ki
Edge length
B
Width (reference: reference edge Z)
C
Q
I
 B<0: Surface in negative Z direction
 B>0: Surface in positive Z direction
Spindle angle of surface normal (default: "C" from section code)
Number of sides (Q >= 2)
Limit diameter (as cutting limit)
 No input: "X" from section code
 "I" overwrites "X" from section code
Whether the surface lies on the front face or rear side has
no effect on the evaluation of the algebraic sign for "width
B."
512
DIN programming for the Y axis
6.3 Contours in the YZ plane
6.3 Contours in the YZ plane
Starting point of contour in YZ plane G180-Geo
G180 defines the starting point of a contour in the YZ plane.
Parameters
Y
Starting point of contour
Z
Starting point of contour
PZ
Starting point of contour (polar radius)
W
Starting point of contour (polar angle)
Line segment in YZ plane G181-Geo
G181 defines a line segment in a contour of the YZ plane.
Parameters
Y
End point
Z
End point
AN Angle to positive Z axis
Q
Point of intersection. End point if the line segment intersects a
circular arc (default: 0):
BR
PZ
W
AR
R
 0: Near point of intersection
 1: Far point of intersection
Chamfer/rounding. Defines the transition to the next contour
element. When entering a chamfer/rounding, program the
theoretical end point.
 No entry: Tangential transition
 BR=0: No tangential transition
 BR>0: Radius of rounding
 BR<0: Width of chamfer
End point (polar radius; reference: workpiece zero point)
End point (polar angle; reference: workpiece zero point)
Angle to positive Z axis (AR corresponds to AN)
Length (polar radius; reference: last contour point)
Programming
 Y, Z: Absolute, incremental, modal or "?"
 ANi: Angle to the subsequent element
 ARi: Angle to the previous element
HEIDENHAIN MANUALplus 620, CNC PILOT 640
513
6.3 Contours in the YZ plane
Circular arc in YZ plane G182-Geo/G183-Geo
G182/G183 defines a circular arc in a contour of the YZ plane. Direction
of rotation: See help graphic
Parameters
Y
End point (radius)
Z
End point
R
Radius
J
Center (Y direction)
K
Center (Z direction)
Q
Point of intersection. End point if the circular arc intersects a
line segment or another circular arc (default: 0):
BR
 0: Near point of intersection
 1: Far point of intersection
Chamfer/rounding. Defines the transition to the next contour
element. When entering a chamfer/rounding, program the
theoretical end point.
 No entry: Tangential transition
 BR=0: No tangential transition
 BR>0: Radius of rounding
 BR<0: Width of chamfer
PZ
End point (polar radius; reference: workpiece zero point)
W
End point (polar angle; reference: workpiece zero point)
PM Center point (polar radius; reference: workpiece zero point)
WM Center point (polar angle; reference: workpiece zero point)
AR Starting angle (tangential angle to rotary axis)
AN End angle (tangential angle to rotary axis)
Programming
 Y, Z: Absolute, incremental, modal or "?"
 J, K: Absolute or incremental
 PZ, W, PM, WM: Absolute or incremental
 ARi: Angle to the previous element
 ANi: Angle to the subsequent element
 End point must not be the starting point (no full circle).
514
DIN programming for the Y axis
6.3 Contours in the YZ plane
Hole in YZ plane G380-Geo
G380 defines a single hole with countersinking and thread in the YZ
plane.
Parameters
Y
Center of hole
Z
Center of hole
B
Hole diameter
P
Depth of hole (excluding point)
W
Point angle (default: 180°)
R
Sinking diameter
U
Sinking depth
E
Sinking angle
I
Thread diameter
J
Thread depth
K
Start of thread (runout length)
F
Thread pitch
V
Left-hand or right-hand thread (default: 0)
A
O
 0: Right-hand thread
 1: Left-hand thread
Angle to X axis (range: –90° < A < 90°)
Centering diameter
Linear slot in YZ plane G381-Geo
G381 defines the contour of a linear slot in the YZ plane.
Parameters
Y
Center of slot
Z
Center of slot
X
Reference diameter
A
K
B
P
 No input: "X" from section code
 "X" overwrites "X" from section code
Position angle (reference: positive Z axis; default: 0°)
Slot length
Slot width
Pocket depth (default: "P" from G308)
HEIDENHAIN MANUALplus 620, CNC PILOT 640
515
6.3 Contours in the YZ plane
Circular slot in YZ plane G382-Geo/G383-Geo
G382/G383 defines a circular slot in the YZ plane.
 G382: Circular slot clockwise
 G383: Circular slot counterclockwise
Parameters
Y
Center of slot curvature
Z
Center of slot curvature
X
Reference diameter
R
A
W
B
P
 No input: "X" from section code
 "X" overwrites "X" from section code
Radius (reference: center point path of the slot)
Starting angle (reference: X axis; default: 0°)
End angle (reference: X axis; default: 0°)
Slot width
Pocket depth (default: "P" from G308)
Full circle in YZ plane G384-Geo
G384 defines a full circle in the YZ plane.
Parameters
Y
Center of circle
Z
Center of circle
X
Reference diameter
R
P
516
 No input: "X" from section code
 "X" overwrites "X" from section code
Circle radius
Pocket depth (default: "P" from G308)
DIN programming for the Y axis
6.3 Contours in the YZ plane
Rectangle in YZ plane G385-Geo
G385 defines a rectangle in the YZ plane.
Parameters
Y
Center of rectangle
Z
Center of rectangle
X
Reference diameter
A
K
B
R
 No input: "X" from section code
 "X" overwrites "X" from section code
Position angle (reference: positive Z axis; default: 0°)
Length of rectangle
Width of rectangle
Chamfer/rounding (default: 0)
P
 R>0: Radius of rounding
 R<0: Width of chamfer
Pocket depth (default: "P" from G308)
Eccentric polygon in YZ plane G387-Geo
G387 defines the contour of an eccentric polygon in the YZ plane.
Parameters
Y
Center point of polygon
Z
Center point of polygon
X
Reference diameter
Q
A
K
 No input: "X" from section code
 "X" overwrites "X" from section code
Number of corners (Q >= 3)
Position angle (reference: positive Z axis; default: 0°)
Edge length / width across flats
R
 K>0: Edge length
 K<0: Width across flats (inside diameter)
Chamfer/rounding—default: 0
P
 R>0: Radius of rounding
 R<0: Width of chamfer
Pocket depth (default: "P" from G308)
HEIDENHAIN MANUALplus 620, CNC PILOT 640
517
6.3 Contours in the YZ plane
Linear pattern in YZ plane G481-Geo
G481 defines a linear pattern in the YZ plane. G481 is effective for the
figure defined in the following block (G380 to G385, G387).
Parameters
Q
Number of figures
Y
1st point of pattern
Z
1st point of pattern
J
End point of pattern (Y direction)
K
End point of pattern (Z direction)
Ji
Distance between two figures (in Y direction)
Ki
Distance between two figures (in Z direction)
A
Position angle of longitudinal axis of pattern (reference:
positive Z axis)
R
Length (overall length of pattern)
Ri
Pattern distance (distance between two figures)
Programming notes
 Program the hole/figure in the following block without a
center.
 The milling cycle (MACHINING section) calls the hole/
figure in the following block—not the pattern definition.
518
DIN programming for the Y axis
6.3 Contours in the YZ plane
Circular pattern in YZ plane G482-Geo
G482 defines a circular pattern in the YZ plane. G482 is effective for
the figure defined in the following block (G380 to G385, G387).
Parameters
Q
Number of figures
K
Diameter (pattern diameter)
A
Starting angle—position of the first figure; reference: Z axis;
(default: 0°)
W
End angle—position of the last figure; reference: Z axis;
(default: 360°)
Wi
Angle between two figures
V
Direction—orientation (default: 0)
Y
Z
H
 V=0, without W: Figures are arranged on a full circle
 V=0, with W: Figures are arranged on the longer circular arc
 V=0, with Wi: The algebraic sign of Wi defines the direction
(Wi<0: clockwise)
 V=1, with W: Clockwise
 V=1, with Wi: Clockwise (algebraic sign of Wi has no effect)
 V=2, with W: Counterclockwise
 V=2, with Wi: Counterclockwise (algebraic sign of Wi has no
effect)
Center of pattern
Center of pattern
Position of the figures (default: 0)
 0: Normal position—the figures are rotated about the circle
center (rotation)
 1: Original position—the position of the figures relative to the
coordinate system remains unchanged (translation)
 Program the hole/figure in the following block without a
center. Exception: circular slot.
 The milling cycle (MACHINING section) calls the hole/
figure in the following block—not the pattern definition.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
519
6.3 Contours in the YZ plane
Single surface in YZ plane G386-Geo
G386 defines a surface in the YZ plane.
Parameters
Z
Reference edge
K
Residual depth
Ki
Depth
B
Width (reference: reference edge Z)
X
 B<0: Surface in negative Z direction
 B>0: Surface in positive Z direction
Reference diameter
C
 No input: "X" from section code
 "X" overwrites "X" from section code
Spindle angle of surface normal (default: "C" from section code)
The reference diameter X limits the surface to be
machined.
Centric polygon in YZ plane G487-Geo
G487 defines polygonal surfaces in the YZ plane.
Parameters
Z
Reference edge
K
Width across flats (inscribed circle diameter)
Ki
Edge length
B
Width (reference: reference edge Z)
X
 B<0: Surface in negative Z direction
 B>0: Surface in positive Z direction
Reference diameter
C
Q
 No input: "X" from section code
 "X" overwrites "X" from section code
Spindle angle of surface normal (default: "C" from section code)
Number of sides (Q >= 2)
The reference diameter X limits the surface to be
machined.
520
DIN programming for the Y axis
6.4 Working planes
6.4 Working planes
Y-axis machining
When programming drilling or milling operations with the Y axis, you
need to define the working plane.
If no working plane is programmed, the Steuerung assumes a turning
operation or a milling operation with the C axis (G18 XZ plane).
G17 XY plane (front or rear face)
Milling cycles are executed in the XY plane, with the depth feed for
milling and drilling cycles in the Z direction.
G18 XZ plane (turning)
In the XZ plane, "normal turning operations" as well as drilling and
milling operations are executed with the C axis.
G19 YZ plane (lateral view / lateral surface)
Milling cycles are executed in the YZ plane, with the depth feed for
milling and drilling cycles in the X direction.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
521
6.4 Working planes
Tilting the working plane G16
G16 executes the following transformations and rotations:
X
X
Plane reference in X direction (radius)
K
Plane reference in Z direction
U
Shift in X direction
W
Shift in Z direction
Q
Enable/disable tilting the working plane
W
B
Parameters
B
Plane angle; reference: positive Z axis
I
U, W
B, I, K
 Shifts the coordinate system to the position I, K
 Rotates the coordinate system by the angle B; reference point: I, K
 Shifts, if programmed, the coordinate system by U and W in the
rotated coordinate system
–U
I
Z
Z
–K
 0: Disable tilted working plane function
 1: Tilt working plane
 2: Restore previous G16 plane
G16 Q0 resets the working plane. The zero point and coordinate
system defined before G16 are then in effect again.
X
X
B
G16 Q2 restores the previous G16 plane.
B
Z
The positive Z axis is the reference axis for the "plane angle B." This
also applies to a mirrored coordinate system.
Z
Please note:
 X is the infeed axis in a tilted coordinate system. X
coordinates are entered as diameter coordinates.
 Mirroring the coordinate system has no effect on the
reference axis of the tilt angle ("B axis angle" of the tool
call).
 Other zero point shifts are not permitted while G16 is
active.
Beispiel: "G16"
...
MACHINING
...
N.. G19
N.. G15 B130
N.. G16 B130 I59 K0 Q1
N.. G1 x.. Z.. Y..
N.. G16 Q0
...
522
DIN programming for the Y axis
6.5 Tool positioning in the Y axis
6.5 Tool positioning in the Y axis
Rapid traverse G0
G0 moves the tool at rapid traverse along the shortest path to the
"target point X, Y, Z."
Parameters
X
Diameter—target point
Z
Length—target point
Y
Length—target point
Programming X, Y, Z: Absolute, incremental or modal
Approach tool change point G14
G14 moves at rapid traverse to the tool change position. In setup
mode, define permanent coordinates for the tool change position.
Parameters
Q
Sequence (default: 0)
 0: Move simultaneously in X and Z axes (diagonal path)
 1: First X, then Z direction
 2: First Z, then X direction
 3: Only X direction, Z remains unchanged
 4: Only Z direction, X remains unchanged
 5: Only Y direction
 6: Move simultaneously in X, Y and Z axes (diagonal path)
If Q=0 to 4, the Y axis does not move.
Rapid traverse to machine coordinates G701
G701 moves the tool at rapid traverse along the shortest path to the
"target point X, Y, Z."
Parameters
X
End point (diameter)
Y
End point
Z
End point
"X, Y, Z" refer to the machine zero point and the slide
reference point.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
523
6.6 Linear and circular movements in the Y axis
6.6 Linear and circular movements
in the Y axis
Milling: Linear movement G1
G1 moves the tool on a linear path at the feed rate to the "end point."
The execution of G1 varies depending on the working plane:
 G17 Interpolation in the XY plane
 Infeed in Z direction
 Angle A—reference: positive X axis
 G18 Interpolation in the XZ plane
 Infeed in Y direction
 Angle A—reference: negative Z axis
 G19 Interpolation in the YZ plane
 Infeed in X direction
 Angle A—reference: positive Z axis
Parameters
X
End point (diameter)
Y
End point
Z
End point
AN Angle (reference: depends on the working plane)
Q
Point of intersection. End point if the circular arc intersects a
line segment or another circular arc (default: 0):
BR
BE
 0: Near point of intersection
 1: Far point of intersection
Chamfer/rounding. Defines the transition to the next contour
element. When entering a chamfer/rounding, program the
theoretical end point.
 No entry: Tangential transition
 BR=0: No tangential transition
 BR>0: Radius of rounding
 BR<0: Width of chamfer
Special feed factor for chamfer/rounding arc (default: 1)
Special feed rate = active feed rate * BE (0 < BE <= 1)
Programming X, Y, Z: Absolute, incremental, modal or "?"
524
DIN programming for the Y axis
6.6 Linear and circular movements in the Y axis
Milling: Circular movement G2, G3—incremental
center coordinates
G2/G3 moves the tool in a circular arc at the feed rate to the "end
point."
The execution of G2/G3 varies depending on the working plane:
 G17 Interpolation in the XY plane
 Infeed in Z direction
 Center definition: with I, J
 G18 Interpolation in the XZ plane
 Infeed in Y direction
 Center definition: with I, K
 G19 Interpolation in the YZ plane
 Infeed in X direction
 Center definition: with J, K
Parameters
X
End point (diameter)
Y
End point
Z
End point
I
Incremental center point (radius)
J
Incremental center point
K
Incremental center point
R
Radius
Q
Point of intersection. End point if the circular arc intersects a
line segment or another circular arc (default: 0):
BR
BE
 0: Near point of intersection
 1: Far point of intersection
Chamfer/rounding. Defines the transition to the next contour
element. When entering a chamfer/rounding, program the
theoretical end point.
 No entry: Tangential transition
 BR=0: No tangential transition
 BR>0: Radius of rounding
 BR<0: Width of chamfer
Special feed factor for chamfer/rounding arc (default: 1)
Special feed rate = active feed rate * BE (0 < BE <= 1)
If you do not program the center, the Steuerung automatically
calculates the possible solutions for the center and chooses that point
as the center which results in the shortest arc.
Programming X, Y, Z: Absolute, incremental, modal or "?"
HEIDENHAIN MANUALplus 620, CNC PILOT 640
525
6.6 Linear and circular movements in the Y axis
Milling: Circular movement G12, G13—absolute
center coordinates
G12/G13 moves the tool in a circular arc at the feed rate to the "end
point."
The execution of G12/G13 varies depending on the working plane:
 G17 Interpolation in the XY plane
 Infeed in Z direction
 Center definition: with I, J
 G18 Interpolation in the XZ plane
 Infeed in Y direction
 Center definition: with I, K
 G19 Interpolation in the YZ plane
 Infeed in X direction
 Center definition: with J, K
Parameters
X
End point (diameter)
Y
End point
Z
End point
I
Absolute center point (radius)
J
Absolute center point
K
Absolute center point
R
Radius
Q
Point of intersection. End point if the line segment intersects a
circular arc (default: 0):
B
E
 Q=0: Near point of intersection
 Q=1: Far point of intersection
Chamfer/rounding. Defines the transition to the next contour
element. When entering a chamfer/rounding, program the
theoretical end point.
 No entry: Tangential transition
 B=0: No tangential transition
 B>0: Radius of rounding
 B<0: Width of chamfer
Special feed factor for the chamfer/rounding arc (default: 1)
Special feed rate = active feed rate * E (0 < E <= 1)
If you do not program the center, the Steuerung automatically
calculates the possible solutions for the center and chooses that point
as the center which results in the shortest arc.
Programming X, Y, Z: Absolute, incremental, modal or "?"
526
DIN programming for the Y axis
6.7 Milling cycles for the Y axis
6.7 Milling cycles for the Y axis
Area milling—roughing G841
G841 roughs surfaces defined with G376-Geo (XY plane) or with
G386-Geo (YZ plane). The cycle mills from the outside toward the
inside. The tool moves to the working plane outside of the workpiece
material.
Parameters
ID
Milling contour—name of the contour to be milled
NS Block number—reference to the contour description
P
Milling depth (maximum infeed in the working plane)
I
Oversize in X direction
K
Oversize in Z direction
U
(Minimum) overlap factor. Defines the overlap of milling paths
(default: 0.5).
V
F
RB
Overlap = U*milling diameter
Overrun factor. Defines the distance by which the tool should
pass the outside radius of the workpiece (default: 0.5).
Overrun = V*milling diameter
Feed rate for infeed (default: active feed rate)
Retraction plane (default: back to starting position)
 XY plane: Retraction position in Z direction
 YZ plane: Retraction position in X direction (diameter)
Oversizes are taken into account:
 G57: Oversize in X and Z direction
 G58: Equidistant oversize in the milling plane
Cycle run
1
Starting position (X, Y, Z, C) is the position before the cycle
begins.
2
Calculate the proportioning of cuts (infeeds to the milling planes,
infeeds in the milling depths).
3
Move to the safety clearance and plunge to the first milling depth.
4
Mill the first plane.
5
Retract by the safety clearance, return and cut to the next milling
depth.
6
Repeat steps 4 and 5 until the complete area is milled.
7
Return to retraction plane RB.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
527
6.7 Milling cycles for the Y axis
Area milling—finishing G842
G842 finishes surfaces defined with G376-Geo (XY plane) or G386Geo (YZ plane). The cycle mills from the outside toward the inside. The
tool moves to the working plane outside of the workpiece material.
Parameters
ID
Milling contour—name of the contour to be milled
NS
Block number—reference to the contour description
P
Milling depth (maximum infeed in the working plane)
H
Cutting direction for side finishing (default: 0)
U
V
F
RB
 H=0: Up-cut milling
 H=1: Climb milling
(Minimum) overlap factor. Defines the overlap of milling paths
(default: 0.5).
Overlap = U*milling diameter
Overrun factor. Defines the distance by which the tool should
pass the outside radius of the workpiece (default: 0.5).
Overrun = V*milling diameter
Feed rate for infeed (default: active feed rate)
Retraction plane (default: back to starting position)
 XY plane: Retraction position in Z direction
 YZ plane: Retraction position in X direction (diameter)
Cycle run
1
Starting position (X, Y, Z, C) is the position before the cycle
begins.
2
Calculate the proportioning of cuts (infeeds to the milling planes,
infeeds in the milling depths).
3
Move to the safety clearance and plunge to the first milling depth.
4
Mill the first plane.
5
Retract by the safety clearance, return and cut to the next milling
depth.
6
Repeat steps 4 and 5 until the complete area is milled.
7
Return to retraction plane RB.
528
DIN programming for the Y axis
6.7 Milling cycles for the Y axis
Centric polygon milling—roughing G843
G843 roughs centric polygons defined with G477-Geo (XY plane) or
G487-Geo (YZ plane). The cycle mills from the outside toward the
inside. The tool moves to the working plane outside of the workpiece
material.
Parameters
ID
Milling contour—name of the contour to be milled
NS Block number—reference to the contour description
P
Milling depth (maximum infeed in the working plane)
I
Oversize in X direction
K
Oversize in Z direction
U
(Minimum) overlap factor. Defines the overlap of milling paths
(default: 0.5).
V
F
RB
Overlap = U*milling diameter
Overrun factor. Defines the distance by which the tool should
pass the outside radius of the workpiece (default: 0.5).
Overrun = V*milling diameter
Feed rate for infeed (default: active feed rate)
Retraction plane (default: back to starting position)
 XY plane: Retraction position in Z direction
 YZ plane: Retraction position in X direction (diameter)
Oversizes are taken into account:
 G57: Oversize in X and Z direction
 G58: Equidistant oversize in the milling plane
Cycle run
1
Starting position (X, Y, Z, C) is the position before the cycle
begins.
2
Calculate the proportioning of cuts (infeeds to the milling planes,
infeeds in the milling depths) and the spindle positions.
3
Spindle turns to the first position. The tool moves to the safety
clearance and plunges to the first milling depth.
4
Mill the first plane.
5
Retract by the safety clearance, return and cut to the next milling
depth.
6
Repeat steps 4 and 5 until the complete area is milled.
7
The tool returns to "retraction plane J." The spindle turns to the
next position. The tool moves to the safety clearance and plunges
to the first milling depth.
8
Repeat steps 4 to 7 until all polygonal surfaces are milled.
9
Return to retraction plane RB.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
529
6.7 Milling cycles for the Y axis
Centric polygon milling—finishing G844
G844 finishes centric polygons defined with G477-Geo (XY plane) or
with G487-Geo (YZ plane). The cycle mills from the outside toward the
inside. The tool moves to the working plane outside of the workpiece
material.
Parameters
ID
Milling contour—name of the contour to be milled
NS
Block number – reference to contour description
P
Milling depth (maximum infeed in the working plane)
H
Cutting direction for side finishing (default: 0)
U
V
F
RB
 H=0: Up-cut milling
 H=1: Climb milling
(Minimum) overlap factor. Defines the overlap of milling paths
(default: 0.5).
Overlap = U*milling diameter
Overrun factor. Defines the distance by which the tool should
pass the outside radius of the workpiece (default: 0.5).
Overrun = V*milling diameter
Feed rate for infeed (default: active feed rate)
Retraction plane (default: back to starting position)
 XY plane: Retraction position in Z direction
 YZ plane: Retraction position in X direction (diameter)
Cycle run
1
Starting position (X, Y, Z, C) is the position before the cycle
begins.
2
Calculate the proportioning of cuts (infeeds to the milling planes,
infeeds in the milling depths) and the spindle positions.
3
Spindle turns to the first position. The tool moves to the safety
clearance and plunges to the first milling depth.
4
Mill the first plane.
5
Retract by the safety clearance, return and cut to the next milling
depth.
6
Repeat steps 4 and 5 until the complete area is milled.
7
The tool returns to "retraction plane J." The spindle turns to the
next position. The tool moves to the safety clearance and plunges
to the first milling depth.
8
Repeat steps 4 to 7 until all polygonal surfaces are milled.
9
Return to retraction plane RB.
530
DIN programming for the Y axis
6.7 Milling cycles for the Y axis
Pocket milling—roughing G845 (Y axis)
G845 roughs closed contours that are defined in the XY or YZ plane in
the program sections:
 FACE_Y
 REAR_Y
 LATERAL_Y
Choose one of the following plunge strategies, depending on the
milling cutter you are using:
 Plunge vertically
 Plunge at a pre-drilled position
 Plunge in a reciprocating or helical motion
When "plunging at a pre-drilled position," you have the following
alternatives:
 Calculate positions, drill, mill. The machining process is
performed in the following steps:
 Insert drill.
 Calculate hole positions with "G845 A1 ..."
 Drill holes with "G71 NF ..."
 Call cycle "G845 A0 ..." The cycle positions the tool above the hole;
the tool plunges and mills the pocket.
 Drill, mill. The machining process is performed in the following
steps:
 Drill a hole inside the pocket with "G71 ..."
 Position the milling cutter above the hole and call "G845 A0 ..." The
tool plunges and mills the section.
If the pocket consists of multiple sections, G845 takes all the sections
of the pocket into account for drilling and milling. Call "G845 A0 .."
separately for each section when calculating the hole positions
without "G845 A1 ..".
G845 takes the following oversizes into account:
 G57: Oversize in X and Z direction
 G58: Equidistant oversize in the milling plane
Program oversizes for calculating the hole positions and
for milling.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
531
6.7 Milling cycles for the Y axis
G845 (Y axis)—Calculating hole positions
"G845 A1 .." calculates the hole positions and stores them at the
reference specified in "NF." The cycle takes the diameter of the active
tool into account when calculating the hole positions. Therefore, you
need to insert the drill before calling "G845 A1 ..". Program only the
parameters given in the following table.
See also:
 G845—Fundamentals: Page 531
 G845—Milling: Page 533
Parameters—Calculating hole positions
ID
Milling contour—name of the contour to be milled
NS
Starting block no. of contour
B
XS
ZS
I
K
Q
A
NF
WB
 Figures: Block number of the figure
 Free closed contour: A contour element (not starting point)
Milling depth (default: depth from the contour description)
Milling top edge—lateral surface (replaces the reference plane
from the contour definition)
Milling top edge—face (replaces the reference plane from the
contour definition)
Oversize in X direction (radius)
Oversize in Z direction
Machining direction (default: 0)
 0: From the inside out (from the inside towards the outside)
 1: From the outside in (from the outside towards the inside)
Sequence for "Calculate hole positions": A=1
Position mark—reference at which the cycle stores the hole
positions [1 to 127].
(Plunging length) Diameter of the milling cutter
 G845 overwrites any hole positions that may still be
stored at the reference "NF."
 The parameter "WB" is used both for calculating the hole
positions and for milling. When calculating the hole
positions, "WB" describes the diameter of the milling
cutter.
532
DIN programming for the Y axis
6.7 Milling cycles for the Y axis
G845 (Y axis)—Milling
You can change the cutting direction with the "cutting direction H,"
the "machining direction Q" and the direction of tool rotation (see table
G845 in the User's Manual). Program only the parameters given in the
following table.
See also:
 G845—Fundamentals: Page 531
 G845—Calculating hole positions: Page 532
Parameters—Milling
ID
Milling contour—name of the contour to be milled
NS Starting block no. of contour
B
P
XS
ZS
I
K
U
V
H
 Figures: Block number of the figure
 Free closed contour: A contour element (not starting point)
Milling depth (default: depth from the contour description)
Maximum infeed (default: milling in one infeed)
Milling top edge in YZ plane (replaces the reference diameter
from the contour description)
Milling top edge in XY plane (replaces the reference plane from
the contour description)
Oversize in X direction (radius)
Oversize in Z direction
(Minimum) overlap factor. Defines the overlap of milling paths
(default: 0.5).
Overlap = U*milling diameter
Overrun factor (default: 0.5. Defines the distance by which the
tool should pass the outside radius of the workpiece.
 0: The defined contour is milled completely
 0<V<=1: Overrun = V*milling diameter
Cutting direction (default: 0)
RB
 0: Up-cut milling
 1: Climb milling
Feed rate for infeed (default: active feed rate)
Reduced feed rate for circular elements (default: current feed
rate)
Retraction plane (default: back to starting position)
Q
 XY plane: Retraction position in Z direction
 YZ plane: Retraction position in X direction (diameter)
Machining direction (default: 0)
F
E
A
NF
 0: From the inside out (from the inside towards the outside)
 1: From the outside in (from the outside towards the inside)
Sequence for "Milling": A=0 (default=0)
Position mark—reference from which the cycle reads the hole
positions [1 to 127].
HEIDENHAIN MANUALplus 620, CNC PILOT 640
533
6.7 Milling cycles for the Y axis
Parameters—Milling
O
Plunging behavior (default: 0)
O=0 (vertical plunge): The cycle moves the tool to the starting
point; the tool plunges at the feed rate for infeed and mills the
pocket.
O=1 (plunge at pre-drilled position):
 If "NF" is programmed: The cycle positions the milling cutter
above the first pre-drilled hole; the tool plunges and mills the
first area. If applicable, the cycle positions the tool to the
next pre-drilled hole and mills the next area, etc.
 If "NF" is not programmed: The tool plunges at the current
position and mills the area. If applicable, position the tool to
the next pre-drilled hole and mill the next area, etc.
O=2, 3 (helical plunge): The tool plunges at the angle "W" and
mills full circles with the diameter "WB." As soon as it reaches
the milling depth "P," the cycle switches to face milling.
 O=2—manually: The cycle plunges at the current position
and machines the area that can be reached from this
position.
 O=3—automatically: The cycle calculates the plunging
position, plunges and machines this area. The plunging
motion ends at the starting point of the first milling path, if
possible. If the pocket consists of multiple areas, the cycle
successively machines all the areas.
O=4, 5 (reciprocating linear plunge): The tool plunges at the
angle "W" and mills a linear path of the length "WB." You can
define the orientation angle in "WE." The cycle then mills along
this path in the opposite direction. As soon as it reaches the
milling depth "P," the cycle switches to face milling.
 O=4—manually: The cycle plunges at the current position
and machines the area that can be reached from this
position.
 O=5—automatically: The cycle calculates the plunging
position, plunges and machines this area. The plunging
motion ends at the starting point of the first milling path, if
possible. If the pocket consists of multiple areas, the cycle
successively machines all the areas. The plunging position is
determined from the type of figure and from "Q" as follows:
 Q0 (from the inside toward the outside):
– Linear slot, rectangle, polygon: Reference point of the
figure
– Circle: Circle center
– Circular slot, "free" contour: Starting point of the
innermost milling path
 Q1 (from the outside toward the inside):
– Linear slot: Starting point of the slot
– Circular slot, circle: Not machined
– Rectangle, polygon: Starting point of the first linear
element
– "Free" contour: Starting point of the first linear element
(at least one linear element must exist)
534
DIN programming for the Y axis
W
WE
6.7 Milling cycles for the Y axis
Parameters—Milling
O=6, 7 (reciprocating circular plunge): The tool plunges at
the plunging angle "W" and mills a circular arc of 90°. The cycle
then mills along this path in the opposite direction. As soon as
it reaches the milling depth "P," the cycle switches to face
milling. "WE" defines the arc center, "WB" the arc radius.
 O=6—manually: The tool position corresponds to the center
of the circular arc. The tool moves to the arc starting point
and plunges.
 O=7—automatically (only permitted for circular slots and
circles): The cycle calculates the plunging position on the
basis of "Q":
 Q0 (from the inside toward the outside):
– Circular slot: The circular arc lies on the curvature radius
of the slot
– Circle: Not permitted
 Q1 (from the outside toward the inside): Circular slot,
circle: The circular arc lies on the outermost milling path
Plunging angle in infeed direction
Orientation angle of the milling path/circular arc. Reference
axis:
 Front or rear face: Positive XK axis
 Lateral surface: Positive Z axis
Default orientation angle, depending on "O":
WB
 O=4: WE=0°
 O=5 and
 Linear slot, rectangle, polygon: WE= orientation angle of
the figure
 Circular slot, circle: WE=0°
 "Free" contour and Q0 (from the inside toward the
outside): WE=0°
 "Free" contour and Q1 (from the outside toward the
inside): Orientation angle of the starting element
Plunge length/plunge diameter (default: 1.5 * milling diameter)
HEIDENHAIN MANUALplus 620, CNC PILOT 640
535
6.7 Milling cycles for the Y axis
For the cutting direction, machining direction and direction of tool
rotation, please refer to table G845 in the User's Manual.
For the machining direction Q=1 (from the outside toward
the inside), please note:
 The contour must start with a linear element.
 If the starting element is < WB, WB is reduced to the
length of the starting element.
 The length of the starting element must not be less than
1.5 times the diameter of the milling cutter.
Cycle run
1
Starting position (X, Y, Z, C) is the position before the cycle
begins.
2
Calculate the number of cuts (infeeds to the milling planes,
infeeds in the milling depths) and the plunging positions and
paths for reciprocating or helical plunges.
3
Approach to safety clearance and, depending on O, feed to the
first milling depth or approach helically or on a reciprocating path.
4
Mill a plane.
5
Retract by the safety clearance, return and cut to the next milling
depth.
6
Repeat steps 4 and 5 until the complete surface is milled.
7
Return to retraction plane RB.
536
DIN programming for the Y axis
6.7 Milling cycles for the Y axis
Pocket milling—finishing G846 (Y axis)
G846 finishes closed contours defined in the XY or YZ plane in the
program sections:
 FACE_Y
 REAR_Y
 LATERAL_Y
You can change the cutting direction with the "cutting direction H,"
the "machining direction Q" and the direction of tool rotation.
Parameters—finishing
ID
Milling contour—name of the contour to be milled
NS Starting block no. of contour
B
P
XS
ZS
R
U
V
H
 Figures: Block number of the figure
 Free closed contour: A contour element (not starting point)
Milling depth (default: depth from the contour description)
Maximum infeed (default: milling in one infeed)
Milling top edge in YZ plane (replaces the reference diameter
from the contour description)
Milling top edge in XY plane (replaces the reference plane from
the contour description)
Radius of approaching/departing arc (default: 0)
 R=0: Contour element is approached directly. Feed to the
starting point above the milling plane, then vertical plunge.
 R>0: Tool moves on approaching/departing arc that
connects tangentially to the contour element.
(Minimum) overlap factor. Defines the overlap of milling paths
(default: 0.5).
Overlap = U*milling diameter
Overrun factor—no effect with C-axis machining
Cutting direction (default: 0)
RB
 0: Up-cut milling
 1: Climb milling
Feed rate for infeed (default: active feed rate)
Reduced feed rate for circular elements (default: current feed
rate)
Retraction plane (default: back to starting position)
Q
 XY plane: Retraction position in Z direction
 YZ plane: Retraction position in X direction (diameter)
Machining direction (default: 0)
F
E
 0: From the inside out (from the inside towards the outside)
 1: From the outside in (from the outside towards the inside)
HEIDENHAIN MANUALplus 620, CNC PILOT 640
537
6.7 Milling cycles for the Y axis
Parameters—finishing
O
Plunging behavior (default: 0)
 O=0 (vertical plunge): The cycle moves the tool to the
starting point; the tool plunges and finishes the pocket.
 Q=1 (approaching arc with depth feed): When machining the
upper milling planes, the tool advances to the milling plane
and then approaches on an arc. When machining the bottom
milling plane, the tool plunges to the milling depth while
moving on the approaching arc (three-dimensional
approaching arc). You can use this approach behavior only in
conjunction with an approaching arc "R" and when machining
from the outside toward the inside (Q=1).
For the cutting direction, machining direction and direction of tool
rotation, please refer to table G846 in the User's Manual.
Cycle run
1
Starting position (X, Y, Z, C) is the position before the cycle
begins.
2
Calculate the proportioning of cuts (infeeds to the milling planes,
infeeds in the milling depths).
3
Move to the safety clearance and plunge to the first milling depth.
4
Mill the first plane.
5
Retract by the safety clearance, return and cut to the next milling
depth.
6
Repeat steps 4 and 5 until the complete area is milled.
7
Return to "retraction plane J."
538
DIN programming for the Y axis
6.7 Milling cycles for the Y axis
Engraving in XY plane G803
G803 engraves character strings aligned linearly in the XY plane.
Character set: see page 376
The cycles start engraving from the starting position or from the
current position, if no starting position is defined.
Example: If a character string is engraved with several calls, define the
starting position in the first call. All other calls are programmed without
a starting position.
Parameters
X, Y Starting point
Z
End point. Z position, infeed depth during milling.
RB
Retraction plane. Z position retracted to for positioning.
ID
Text to be engraved
NF
Character number (character to be engraved)
W
Orientation angle of the character string. Example: 0° =
Vertical characters: the characters are aligned in sequence in
positive X direction
H
Font height
E
Distance factor (for calculation see figure)
F
Plunging feed rate factor (plunging feed rate = current feed
rate * F)
HEIDENHAIN MANUALplus 620, CNC PILOT 640
539
6.7 Milling cycles for the Y axis
Engraving in the YZ plane G804
The cycles start engraving from the starting position or from the
current position, if no starting position is defined.
Example: If a character string is engraved with several calls, define the
starting position in the first call. All other calls are programmed without
a starting position.
G804 engraves character strings aligned linearly in the YZ plane.
Character set: see page 376
Parameters
Y, Z Starting point
X
End point (diameter). X position, infeed depth during milling.
RB Retraction plane. X position retracted to for positioning.
ID
Text to be engraved
NF
Character number. ASCII code of the character to be engraved
H
Font height
E
Distance factor (for calculation see figure)
E
Distance factor. The distance between the characters is
calculated according to the following formula: H / 6 * E
F
Plunging feed rate factor (plunging feed rate = current feed
rate * F)
540
DIN programming for the Y axis
6.7 Milling cycles for the Y axis
Thread milling in XY plane G800
G800 mills a thread in existing holes.
Place the tool on the center of the hole before calling G799. The cycle
positions the tool on the end point of the thread within the hole. Then
the tool approaches on "approach radius R" and mills the thread. During
this, the tool advances by the thread pitch F. Following that, the cycle
retracts the tool and returns it to the starting point. With parameter V,
you can program whether the thread is to be milled in one rotation or,
with single-point tools, in several rotations.
Parameters
I
Thread diameter
Z
Starting point Z
K
Thread depth
R
Approach radius
F
Thread pitch
J
Direction of thread (default: 0)
H
 0: Right-hand thread
 1: Left-hand thread
Cutting direction (default: 0)
V
 0: Up-cut milling
 1: Climb milling
Milling method
 0: The thread is milled in a 360-degree helix
 1: The thread is milled in several helical paths (single-point
tool)
Use thread-milling tools for cycle G800.
Danger of collision!
Be sure to consider the hole diameter and the diameter of
the milling cutter when programming "approach radius R."
HEIDENHAIN MANUALplus 620, CNC PILOT 640
541
6.7 Milling cycles for the Y axis
Thread milling in YZ plane G806
G806 mills a thread in existing holes.
Place the tool on the center of the hole before calling G799. The cycle
positions the tool on the end point of the thread within the hole. Then
the tool approaches on "approach radius R" and mills the thread. During
this, the tool advances by the thread pitch F. Following that, the cycle
retracts the tool and returns it to the starting point. With parameter V,
you can program whether the thread is to be milled in one rotation or,
with single-point tools, in several rotations.
Parameters
I
Thread diameter
X
Starting point in X
K
Thread depth
R
Approach radius
F
Thread pitch
J
Direction of thread (default: 0)
H
 0: Right-hand thread
 1: Left-hand thread
Cutting direction (default: 0)
V
 0: Up-cut milling
 1: Climb milling
Milling method
 0: The thread is milled in a 360-degree helix
 1: The thread is milled in several helical paths (single-point
tool)
Use thread-milling tools for cycle G806.
Danger of collision!
Be sure to consider the hole diameter and the diameter of
the milling cutter when programming "approach radius R."
542
DIN programming for the Y axis
6.7 Milling cycles for the Y axis
Hobbing G808
G808 mills a gear profile from the "starting point in Z" to the "end point
K". In W you enter the angular position of the tool.
If an oversize has been programmed, hobbing is split up in roughmachining and subsequent finishing.
In parameters O, R and V you define the tool shift. Shifting by R
ensures a uniform wear of the hob cutter.
Parameters
Z
Starting point
K
End point
C
Angle (offset angle of the C axis)
A
Root circle diameter
B
Outside diameter
J
Number of workpiece teeth
W
Angular position
S
Surface speed [m/min]
I
Oversize
D
Direction of rotation of the workpiece
 3: M3
 4: M4
F
Feed per revolution
E
Finishing feed rate
P
Maximum infeed
O
Shift starting position
R
Shift value
V
Number of shifts
H
Infeed axis
 0: Tool infeed is performed in the X axis
 1: Tool infeed is performed in the Y axis
Q
Workpiece spindle
 0: Spindle no. 0 (main spindle) holds the workpiece
 3: Spindle no. 3 (opposing spindle) holds the workpiece
HEIDENHAIN MANUALplus 620, CNC PILOT 640
543
6.8 Example program
6.8 Example program
Machining with the Y axis
The milling and drilling contours are nested in the following NC
program. A linear slot is machined on the single surface. On the same
single surface, a hole pattern with two holes is machined both to the
left and right of the slot.
At first, the turning operation is performed, and then the single surface
is milled. Following that, the linear slot is machined using the "Pocket
milling, lateral surface Y" unit. Then the slot is deburred. Further units
are used to center the hole patterns, then drill them and finally tap the
holes.
544
DIN programming for the Y axis
6.8 Example program
Example: "Y axis [BSP_Y.NC]"
HEADER
#MATERIAL
Aluminum
#WORKPIECE
Example Y axis
#MEASURE_UNITS Metric
TURRET 1
T1
ID"Roughing 80 G."
T2
ID"NC center drill"
T3
ID"Finishing 35 G."
T4
ID"Drill 5.2mm"
T5
ID"Thread outside"
T6
ID"Tapping M6"
T8
ID"Mill D16mm"
T10
ID"Mill D6mm"
T12
ID"Deburring_m"
BLANK
N
1 G20 X70 Z97 K1
FINISHED
N
2 G0 X0 Z0
N
3 G1 X30 BR-2
N
4 G1 Z-20
N
5 G25 H7 I1.5 K7 R1 W30 FP2
N
6 G1 X56 BR-1
N
7 G1 Z-60
N
8 G1 X64 BR-1
N
9 G1 Z-75 BR-1
[Undercut DIN 76]
N 10 G1 X44 BR3
N 11 G1 Z-95 BR-1
N 12 G1 X0
N 13 G1 Z0
LATERAL_Y X56 C0
[Define YZ plane]
N 14 G308 ID"Surface"
N 15
G386 Z-55 Ki8 B30 X56 C0
N 16
G308 ID"Slot 10mm" P-2
N 17
G381 Z-40 Y0 A90 K50 B10
HEIDENHAIN MANUALplus 620, CNC PILOT 640
[Single surface]
[Linear slot on single surface]
545
6.8 Example program
N 18
G309
N 19
G308 ID"Hole_1 M6" P-15
N 20
G481 Q2 Z-30 Y15 K-30 J-15
[Linear pattern on single surface]
N 21
G380 B5.2 P15 W118 I6 J10 F1 V0 o7
[Drilling, tapping, centering]
N 22
G309
N 23
G308 ID"Hole_2 M6" P-15
N 24
G481 Q2 Z-50 Y15 K-50 J-15
[Linear pattern on single surface]
N 25
G380 B5.2 P15 W118 I6 J10 F1 V0 O7
[Drilling, tapping, centering]
N 26
G309
N 27 G309
MACHINING
N 28 UNIT ID"START"
N 30
G26 S3500
N 31
G126 S2000
N 32
G59 Z256
N 33
G140 D1 X400 Y0 Z500
N 34
G14 Q0 D1
[Start of program]
N 35 END_OF_UNIT
N 36 UNIT ID"G820_ICP"
N 38
T1
N 39
G96 S220 G95 F0.35 M3
N 40
M8
N 41
G0 X72 Z2
N 42
G47 P2
N 43
G820 NS3 NE3 P2 I0 K0 H0 Q0 V3 D0
N 44
G47 M9
[G820 Transverse roughing, ICP]
N 45 END_OF_UNIT
N 46 UNIT ID"G810_ICP"
N 48
T1
N 49
G96 S220 G95 F0.35 M3
N 50
M8
N 51
G0 X72 Z2
N 52
G47 P2
N 53
G810 NS4 NE9 P3 I0.5 K0.2 H0 Q0 V0 D0
N 54
G14 Q0 D1
546
[G810 Longitudinal roughing, ICP]
DIN programming for the Y axis
6.8 Example program
N 55
G47 M9
N 56 END_OF_UNIT
N 57 UNIT ID"G890_ICP"
N 59
T3
N 60
G96 S260 G95 F0.18 M4
N 61
M8
N 62
G0 X72 Z2
N 63
G47 P2
N 64
G890 NS4 NE9 V1 Q0 H3 O0 B0
N 65
G14 Q0 D1
N 66
G47 M9
[G890 Contouring in ICP]
N 67 END_OF_UNIT
N 68 UNIT ID"G32_MAN"
N 70
[G32 Cylindrical thread, direct]
T5
N 71
G97 S800 M3
N 72
M8
N 73
G0 X30 Z5
N 74
G47 P2
N 75
G32 X30 Z-19 F1.5 BD0 IC8 H0 V0
N 76
G14 Q0 D1
N 77
G47 M9
N 78 END_OF_UNIT
N 79 UNIT ID"C_AXIS_ON"
N 81
M14
N 82
G110 C0
[C axis on]
N 83 END_OF_UNIT
N 84 UNIT ID"G841_Y_MANT"
N 86
[Single surface in Y axis, latrl.]
T8
N 87
G197 S1200 G195 F0.25 M104
N 88
M8
N 89
G19
N 90
G110 C0
N 91
G0 Y0
N 92
G0 X74 Z10
HEIDENHAIN MANUALplus 620, CNC PILOT 640
547
6.8 Example program
N 93
G147 K2 I2
N 94
G841 ID"Surface" P5
N 95
G47 M9
N 96
G14 Q0 D1
N 97
G18
[Mill a single surface]
N 98 END_OF_UNIT
N 99 UNIT ID"G845_TAS_Y_MANT"
N 101
T10
N 102
G197 S1200 G195 F0.18 M104
N 103
G19
N 104
M8
N 105
G110 C0
N 106
G0 Y0
N 107
G0 X74 Z-40
N 108
G147 I2 K2
N 109
G845 ID"Slot 10 mm" Q0 H0
N 110
G47 M9
N 111
G14 Q0 D1
N 112
G18
[ICP pocket mill, lateral surf. Y]
[Mill a slot on single surface]
N 113 END_OF_UNIT
N 114 UNIT ID"G840_ENT_Y_MANT"
N 116
T12
N 117
G197 S800 G195 F0.12 M104
N 118
G19
N 119
M8
N 120
G110 C0
N 121
G0 Y0
N 122
G0 X74 Z-40
N 123
G147 I2 K2
N 124
G840 ID"Slot 10mm" Q1 H0 P0.8 B0.15
N 125
G47 M9
N 126
G14 Q0 D1
N 127
G18
[ICP deburring, lateral surf. Y]
[Deburr slot on single surface]
N 128 END_OF_UNIT
N 129 UNIT ID"G72_ICP_Y"
548
[ICP boring, countersinking in Y]
DIN programming for the Y axis
T2
N 132
G197 S1000 G195 F0.22 M104
N 133
M8
N 134
G147 K2
N 135
G72 ID"Hole_1 M6" D0
N 136
G47 M9
6.8 Example program
N 131
[Center the holes of the first pattern]
N 137 END_OF_UNIT
N 138 UNIT ID"G72_ICP_Y"
N 140
T2
N 141
G197 S1000 G195 F0.22 M104
N 142
M8
N 143
G147 K2
N 144
G72 ID"Hole_2 M6" D0
N 145
G47 M9
N 146
G14 Q0 D1
[ICP boring, countersinking in Y]
[Center the holes of the second pattern]
N 147 END_OF_UNIT
N 148 UNIT ID"G74_ICP_Y"
N 150
T4
N 151
G197 S1200 G195 F0.24 M103
N 152
M8
N 153
G147 K2
N 154
G74 ID"Hole_1 M6" D0 V2
N 155
G47 M9
[ICP drilling in Y axis]
[Holes of the first pattern]
N 156 END_OF_UNIT
N 157 UNIT ID"G74_ICP_Y"
N 159
T4
N 160
G197 S1200 G195 F0.24 M103
N 161
M8
N 162
G147 K2
N 163
G74 ID"Hole_2 M6" D0 V2
N 164
G47 M9
N 165
G14 Q0 D1
[ICP drilling in Y axis]
[Holes of the second pattern]
N 166 END_OF_UNIT
N 167 UNIT ID"G73_ICP_Y"
HEIDENHAIN MANUALplus 620, CNC PILOT 640
[ICP tapping in Y axis]
549
6.8 Example program
N 169
T6
N 170
G197 S800 M103
N 171
M8
N 172
G147 K2
N 173
G73 ID"Hole_1 M6" F1
N 174
G47 M9
[Tapping, first pattern]
N 175 END_OF_UNIT
N 176 UNIT ID"G73_ICP_Y"
N 178
T6
N 179
G197 S800 M103
N 180
M8
N 181
G147 K2
N 182
G73 ID"Hole_2 M6" F1
N 183
G47 M9
N 184
G14 Q0 D1
[ICP tapping in Y axis]
[Tapping, second pattern]
N 185 END_OF_UNIT
N 186 UNIT ID"C_AXIS_OFF"
N 188
[C axis off]
M15
N 189 END_OF_UNIT
N 190 UNIT ID"END"
N 192
[Program end]
M30
N 193 END_OF_UNIT
END
550
DIN programming for the Y axis
TURN PLUS
7.1 TURN PLUS mode of operation
7.1
TURN PLUS mode of operation
To create programs with TURN PLUS, you program the blank and
finished part with the aid of interactive graphics. The working plan is
then generated automatically. As a result you get a commented and
structured NC program.
With TURN PLUS you can create NC programs for the following
applications:
 Turning operations
 Drilling and milling with the C axis
 Drilling and milling with the Y axis
TURN PLUS concept
The workpiece description is the basis for working plan generation.
The strategy for generating the working plan is specified in the
machining sequence. The machining parameters define details of
machining. This allows you to adapt TURN PLUS to your individual
needs.
TURN PLUS generates the working plan, which takes technology
attributes such as oversizes, tolerances, etc. into account.
On the basis of the blank form update, TURN PLUS optimizes the
paths for approach and avoids air cuts or collisions between workpiece
and cutting edge.
For tool selection, TURN PLUS uses the tools from the NC program or
from the current turret assignment/magazine list, depending on the
machine parameter settings. If there is no suitable tool in the turret
assignment/magazine list, TURN PLUS looks for a suitable tool in the
tool database.
When clamping the workpiece, TURN PLUS can determine the cutting
limitations and the zero point shift for the NC program, depending on
the machine parameter settings.
The technology database provides the cutting data to TURN PLUS.
Before generating the working plan, please note: The
default values for the machining parameters as well as
general settings are defined in the machine parameters
(see "List of user parameters" in the User's Manual).
552
TURN PLUS
7.2 Automatic working plan generation (AWG)
7.2
Automatic working plan
generation (AWG)
The AWG generates the work blocks of the working plan in the
sequence defined in "Machining sequence." You define the machining
details in the Machining Parameters input form. TURN PLUS
automatically finds all the elements of a work block. Use the
machining sequence editor to specify the machining sequence.
A work block has the following content:
 Tool call
 Cutting values (technology data)
 Approach (may be omitted)
 Machining cycle
 Tool retraction (may be omitted)
 Moving to tool change point (may be omitted)
You can change or supplement the generated work blocks
subsequently.
TURN PLUS simulates the machining in the AWG control graphic. You
can set the sequence and representation of the control graphic via soft
key (see "Graphic simulation" in the User's Manual).
TURN PLUS outputs warnings during the contour analysis
if certain areas cannot be machined at all or not
completely. Check the respective sections after program
creation and adapt them to your needs.
Generating a working plan
After generating the working plan, please note: If no
chucking equipment has been defined in the program as
yet, TURN PLUS defines the chucking equipment for a
specific type of clamping/clamping length and adjusts the
cutting limitation accordingly. Adapt the values in the
finished NC program.
Generating a working plan with TURN PLUS
Select "TURN PLUS." TURN PLUS opens the most recently selected
machining sequence.
Select "AWG." TURN PLUS shows the contours of the
blank and the finished part in the graphics window.
Press the "AWG control graphic" soft key: The AWG
control graphic and program generation are started.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
553
7.2 Automatic working plan generation (AWG)
Press the "Back" soft key to return to the TURN PLUS
menu.
Press the "Back" soft key to switch to smart.Turn.
Use the name of the current program without any
changes and press the "Save" soft key to overwrite
the current program.
Enter a name for the program and confirm with the
"Save" soft key.
Machining sequence—Fundamentals
TURN PLUS analyzes the contour in the sequence defined in
"Machining sequence." In this process the areas to be machined and
the tool parameters are ascertained. The AWG analyzes the contour
using the machining parameters.
TURN PLUS distinguishes between:
 Main machining operation (e.g. Undercutting)
 Submachining operation (e.g. type H, K, or U)
 Machining location (e.g. outside or inside)
"Submachining" and "machining location" refine the machining
specification. If you do not define the submachining operation or
machining location, the AWG generates machining blocks for all
submachining operations/machining locations.
554
TURN PLUS
7.2 Automatic working plan generation (AWG)
The following factors additionally influence the working plan
generation:
 Geometry of the contour
 Attributes of the contour
 Tool availability
 Machining parameters
In the machining sequence you define the sequence in
which the machining steps are carried out. If you only
define the main machining operation in the sequence for a
machining operation, all of the submachining operations
comprised by it are executed in a specific sequence.
However, you can also program the submachining
operations and machining locations individually in any
sequence. In this case you should define the associated
main machining operation again after defining the
submachining operations. This way you can ensure that all
submachining operations and locations are taken into
account.
The machining sequence and the program can be
displayed in a horizontal or vertical window layout. Press
the "Change VIEW" soft key to switch between the two
views.
Press the "Change window" soft key to move the cursor
between the Program and the Machining Sequence
window.
The AWG does not generate the work blocks if any required
preparatory step is missing, or if the appropriate tool is not available,
etc. TURN PLUS skips machining operations/machining sequences
that do not make sense in the machining process.
Organizing machining sequences:
 TURN PLUS always uses the current machining sequence. The
current machining sequence can be edited or overwritten by loading
another machining sequence.
 When you open TURN PLUS, the most recently used machining
sequence is automatically displayed.
Danger of collision!
When executing drilling or milling operations, TURN PLUS
does not check whether the turning operation has already
been completed. Ensure that turning operations precede
drilling or milling operations in the machining sequence.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
555
7.2 Automatic working plan generation (AWG)
Editing and managing machining sequences
TURN PLUS uses the currently active machining sequence. You can
change the machining sequences and adapt them to your range of
parts.
Managing the machining sequence files:
To open the machining sequence:

Select "TURN PLUS > Machining sequence > Open." TURN PLUS
opens the selection list with the machining sequence files.
 Select the desired file.
To save the machining sequence:

Select "TURN PLUS > Machining sequence > Save as." TURN PLUS
opens the selection list with the machining sequence files.
 Enter a new file name or overwrite an existing file.
To create a default machining sequence:


Select "TURN PLUS > Machining sequence > Save HEIDENHAIN
standard as..." TURN PLUS opens the selection list with the
machining sequence files.
Enter a file name under which you wish to store the HEIDENHAIN
default machining sequence.
Editing a machining sequence
Position the cursor
Select "TURN PLUS > Machining sequence > Line." Select the
function.
Inserting a new machining operation
To insert a new machining operation before the cursor position, select
"Insert above the line."
To insert a new machining operation after the cursor position, select
"Insert below the line."
Moving a machining operation
Select "Move line upwards" or "Move line downwards."
556
TURN PLUS
Select "Edit line."
"OK" confirms the new machining sequence.
Deleting a machining operation
"Delete line" deletes the selected machining sequence.
Overview of machining sequences
The following table lists the possible combinations of main machining
operations with submachining operations and machining locations and
explains the working method of the AWG.
Machining sequence for predrilling
Main machining
Submachining
Location
Predrilling
Execution
Contour analysis: Determining the drilling steps
Machining parameter: 3 – Centric predrilling
All
–
Predrilling
Location
Execution
Machining sequence for roughing
Main machining
Submachining
Roughing
Contour analysis: Dividing the contour into areas for longitudinal/
transverse outside machining and longitudinal/transverse inside
machining according to the transverse/longitudinal ratio.
Sequence: First outside, then inside machining
Machining parameter: 4 – Roughing
All
–
Transverse machining, longitudinal machining—outside and inside
Longitudinal
machining
–
Longitudinal machining—outside and inside
Longitudinal
machining
Outside
Longitudinal machining—outside
Longitudinal
machining
Inside
Longitudinal machining—inside
Transverse
machining
–
Transverse machining—outside and inside
Transverse
machining
Outside
Transverse machining—outside
Transverse
machining
Inside
Transverse machining—inside
HEIDENHAIN MANUALplus 620, CNC PILOT 640
557
7.2 Automatic working plan generation (AWG)
Editing the machining sequence
7.2 Automatic working plan generation (AWG)
Main machining
Submachining
Location
Execution
Contour-parallel
–
Contour-parallel machining—outside and inside
Contour-parallel
Outside
Contour-parallel machining—outside
Contour-parallel
Inside
Contour-parallel machining—inside
Machining sequence for finishing
Main machining
Submachining
Location
Finishing
Execution
Contour analysis: Dividing the contour into areas for outside and
inside machining.
Sequence: First outside, then inside machining
Machining parameter: 5 – Finishing
Contour-parallel
–
Outside/inside machining
Contour-parallel
Outside
Outside machining
Contour-parallel
Inside
Inside machining
Location
Execution
Machining sequence for recess turning
Main machining
Submachining
Recess turning
Contour analysis:
 Without previous roughing operation: The complete contour,
including recess areas (undefined recesses), is machined.
 With previous roughing: Recess areas (undefined recesses) are
determined and machined according to the "inward copying
angle (EKW)."
Sequence: First outside, then inside machining
Machining parameter: 1 Global parameters for finished parts
All
–
Radial/axial machining—outside and inside
Longitudinal
machining
Outside
Radial machining—outside
Longitudinal
machining
Inside
Radial machining—inside
Transverse
machining
Outside/
front
Axial machining—outside
Transverse
machining
Inside/front
Axial machining—inside
Recess turning and contour turning are used alternatively.
558
TURN PLUS
Main machining
Submachining
Location
Contour recessing
Execution
Contour analysis: Recess areas (recesses) are determined and
machined according to the "inward copying angle (EKW)."
Sequence: First outside, then inside machining
Machining parameter: 1 Global parameters for finished parts
All
–
Radial/axial machining—outside and inside
Shaft machining: Axial machining on the outside is performed on
front and back
Longitudinal
machining
Outside
Radial machining—outside
Longitudinal
machining
Inside
Radial machining—inside
Transverse
machining
Outside/
front
Axial machining—outside
Transverse
machining
Inside/front
Axial machining—inside
Recess turning and contour turning are used alternatively.
Machining sequence for recessing
Main machining
Submachining
Location
Recessing
Execution
Contour analysis: Determining the "Recess" form elements:
 Type S (guarding ring – recess type S)
 Type D (sealing ring – recess type D)
 Type A (recess general)
 Type FK (relief turn F) – FK is only machined using "Recessing"
if the "inward copying angle (EKW) <= mtw."
Sequence: First outside, then inside machining
Machining parameter (with type FK): 1 Global parameters for
finished parts
All
–
All recess types; radial/axial machining; outside and inside
Type S, D, A, FK
–
Radial/axial machining—outside and inside
Type S, D, A, FK
Outside
Radial machining—outside
Type S, D, A, FK
Inside
Radial machining—inside
Type S, D, A, FK
Outside/
front
Axial machining—outside
Type S, D, A, FK
Inside/front
Axial machining—inside
HEIDENHAIN MANUALplus 620, CNC PILOT 640
559
7.2 Automatic working plan generation (AWG)
Machining sequence for contour recessing
7.2 Automatic working plan generation (AWG)
Machining sequence for undercuts
Main machining
Submachining
Location
Undercutting
Execution
Contour analysis/machining: Determining the "Undercuts" form
elements:
 Type H – Machining using single paths of traverse; copying tool
(type 22x)
 Type K – Machining using single paths of traverse; copying tool
(type 22x)
 Type U – Machining using single paths of traverse; recessing
tool (type 15x)
Sequence: First outside, then inside machining; first radial, then
axial machining
560
All
–
All recess types—outside and inside
All
Outside
All recess types—outside
All
Inside
All recess types—inside
Type H, K, U
–
Radial/axial machining—outside and inside
Type H, K, U
Outside
Machining—outside
Type H, K, U
Inside
Machining—inside
TURN PLUS
Main machining
Submachining
Location
Thread cutting
Execution
Contour analysis: Determining the "Thread" form elements
Sequence: First outside, then inside machining; the elements are
then machined according to the sequence of geometrical
definition
All
–
Machining cylindric (longitudinal), tapered and transverse threads
on the outside and inside of a contour
All
Outside
Machining cylindric (longitudinal), tapered and transverse threads
on the outside of a contour
All
Inside
Machining cylindric (longitudinal), tapered and transverse threads
on the inside of a contour
Cylinder
–
Machining cylindric outside and inside threads
Cylinder
Outside
Machining cylindric outside threads
Cylinder
Inside
Machining cylindric inside threads
Transverse
–
Machining transverse threads on the outside and inside of the
contour
Transverse
Outside
Machining transverse threads on the outside
Transverse
Inside
Machining transverse threads on the inside
Taper
–
Machining taper threads on the outside and inside
Taper
Outside
Machining taper threads on the outside.
Taper
Inside
Machining taper threads on the inside.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
561
7.2 Automatic working plan generation (AWG)
Machining sequence for thread cutting
7.2 Automatic working plan generation (AWG)
Machining sequence for drilling
Main machining
Submachining
Location
Drilling
Execution
Contour analysis: Determining the "Hole" form elements.
Sequence – Drilling operations/drilling combinations:
 Centering / Centering and countersinking
 Drilling
 Countersinking / Drilling and countersinking
 Reaming / Drilling with reaming
 Tapping / Drilling with thread
Sequence – Location:
 Centric
 Front (also machines Y front)
 Lateral surface (also machines Y surface)
– then the elements are machined according to the sequence of
geometrical definition
562
All
–
All drilling/boring operations at all machining locations
All
Centric
Centric machining of all drilling/boring operations
All
Face
All drilling/boring operations on the front face
All
Lateral
All drilling/boring operations on the lateral surface
Centering, drilling,
countersinking,
reaming, tapping
–
Machining at all machining locations
Centering, drilling,
countersinking,
reaming, tapping
Centric
Centric machining on the face
Centering, drilling,
countersinking,
reaming, tapping
Face
Machining on the face
Centering, drilling,
countersinking,
reaming, tapping
Lateral
Machining on the lateral surface
TURN PLUS
Main machining
Submachining
Location
Milling
Execution
Contour analysis: Determining the milling contours.
Sequence – Milling operation:
 Linear and circular slots
 Open contours
 Closed contours (pockets), single surfaces and centric polygons
Sequence – Location:
 Front (also machines Y front)
 Lateral surface (also machines Y surface)
– then the elements are machined according to the sequence of
geometrical definition
All
–
All milling operations at all machining locations
Surface, contour,
slot milling, pocket
Face
All milling operations on the front face
Surface, contour,
slot milling, pocket
Lateral
All milling operations on the lateral surface
Surface, contour,
slot milling, pocket
–
Milling at all machining locations
Surface, contour,
slot milling, pocket
Face
Milling the end face
Surface, contour,
slot milling, pocket
Lateral
Milling on the lateral surface
Location
Execution
Machining sequence for deburring
Main machining
Submachining
Deburring
Contour analysis: Determining milling contours with "Deburring"
attribute.
Sequence – Location:
 Front (also machines Y front)
 Lateral surface (also machines Y surface)
– then the elements are machined according to the sequence of
geometrical definition
All
–
All milling operations at all machining locations
Contour, slot,
pocket (*)
Face
Deburring of all milling operations on the front face
Contour, slot,
pocket (*)
Lateral
Deburring of all milling operations on the lateral surface
HEIDENHAIN MANUALplus 620, CNC PILOT 640
563
7.2 Automatic working plan generation (AWG)
Machining sequence for milling
7.2 Automatic working plan generation (AWG)
Main machining
Submachining
Location
Execution
Contour, slot,
pocket (*)
–
Deburr selected element at all machining locations
Contour, slot,
pocket (*)
Face
Deburr selected element on the face
Contour, slot,
pocket (*)
Lateral
Deburr selected element on the lateral surface
*: Define the type of contour
Machining sequence for milling and finishing
Main machining
Submachining
Location
Finish-milling
Execution
Contour analysis: Determining the milling contours.
Sequence – Milling operation:
 Linear and circular slots
 Open contours
 Closed contours (pockets), single surfaces and centric
polygons
Sequence – Location:
 Front (also machines Y front)
 Lateral surface (also machines Y surface)
– then the elements are machined according to the sequence
of geometrical definition
–
–
Finish-machine all elements at all machining locations
–
Face
Finish-machine all elements on the front face
–
Lateral
Finish-machine all elements on the lateral surface
Contour, slot, pocket
(*)
–
Finish selected element at all machining locations
Contour, slot, pocket
(*)
Face
Finish selected element on the face
Contour, slot, pocket
(*)
Lateral
Finish selected element on the lateral surface
*: Define the milling operation
Machining sequence for parting
Main machining
Submachining
Location
Execution
Parting
All
–
The workpiece is cut off
Full-surface machining
–
The workpiece is cut off and rechucked
564
TURN PLUS
7.2 Automatic working plan generation (AWG)
Machining sequence for rechucking
Main machining
Submachining
Location
Execution
Rechucking
Full-surface machining
–
The workpiece is rechucked.
AWG control graphic
When you create a program with the AWG, the programmed blank
and finished part are displayed in the simulation window and in
addition, all machining steps are simulated successively. The
workpiece blank takes on a contour during machining.
Setting the AWG control graphic
When you start the automatic program creation with the AWG soft
key, the control automatically opens the AWG control graphic. The
simulation displays dialogs in which you get machining and tool
information. After you have simulated the machining process, you can
close the graphics window with the "Back" soft key. The "Save as"
dialog box opens once you exit the TURN PLUS menu with the "Back"
soft key. The name of the opened program is displayed in the "File
name" dialog field. If you do not enter another file name, the opened
program will be overwritten. Alternatively, you can save the machining
operation in another program.
The AWG control graphic is indicated in the soft-key symbol by a
contour outlined in red.
You can set the display of the tool paths and the simulation mode
as usual (see "Graphic simulation" in the User's Manual).
HEIDENHAIN MANUALplus 620, CNC PILOT 640
565
7.3 Machining information
7.3
Machining information
Tool selection, turret assignment
The tool selection is determined by:
 Machining direction
 Contour to be machined
 Machining sequence
 Machine parameter settings, e.g. "Type of tool access" (602001)
If the ideal tool is not available, TURN PLUS
 First looks for a replacement tool,
 Then for an emergency tool.
If necessary, TURN PLUS adapts the machining cycle to the
requirements of the replacement or emergency tool. If more than one
tool is suitable for a machining operation, TURN PLUS uses the
optimal tool. If no tool is found by TURN PLUS, select the tools
manually.
The Mount type distinguishes between different tool holders (see
"Tool editor" in the User's Manual). TURN PLUS checks whether the
mount type in the tool holder description and the mount type in the
turret pocket description are the same.
Depending on the setting of the "Zero point shift" machine
parameter (602022), TURN PLUS automatically calculates
the required zero point shift for the workpiece and
activates it with G59 (see "List of user parameters" in the
User's Manual).
To calculate the zero point shift, TURN PLUS takes the
following values into account:
 Workpiece length Z (description of workpiece blank)
 Oversize K (description of workpiece blank)
 Edge of chuck Z (description of chucking equipment and
machining parameters)
 Edge of chuck B (description of chucking equipment and
machining parameters)
Multipoint tools and manual tool change holders are used
by AWG only if they are already entered in the turret list of
the NC program.
566
TURN PLUS
7.3 Machining information
Manual tool selection
TURN PLUS selects the tools depending on the machining parameter
Type of tool access WD. If TURN PLUS cannot find a suitable tool in
the specified lists, select the tools manually.
TURN PLUS automatically enters comparison parameters. With the
soft keys, you can select the list in which you want to look for the
tools.
Select the "Tool list" soft key
Select the "Turret list" soft key
Choose a tool from the list.
Press the "Take over" soft key to enter the tool in the
tool selection.
Press the "Take over" soft key to conclude the tool
selection.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
567
7.3 Machining information
Contour recessing, recess turning
The cutting radius must be smaller than the smallest inside radius of
the recess contour, but >= 0.2 mm. TURN PLUS determines the
width of the recessing tool from the recess contour:
 Recess contour includes paraxial base elements with radii on both
sides: SB <= b + 2*r (if radii differ: smallest radius).
 Recess contour includes paraxial base elements without radii or
with a radius on one side: SB <= b
 Recess contour does not include paraxial base elements: The width
of the recessing tool is determined from the recessing width divisor
(machining parameter 6 – SBD).
Abbreviations:
 SB: Recessing width
 b: Width of base element
 r: Radius
Drilling
Depending on the geometry of the bore hole, the AWG determines
the appropriate tool. For centric bore holes, TURN PLUS uses
stationary tools.
568
TURN PLUS
7.3 Machining information
Cutting data, coolant
To determine the cutting parameters, TURN PLUS uses the
 Workpiece material (program head)
 Cutting material (tool parameters)
 The machining operation (main operation in the machining
sequence).
The values determined are multiplied by the tool-dependent
compensation factors (see "Tool data" in the User's Manual).
Note for roughing and finishing operations:
 Main feed rate for use of the primary cutting edge
 Auxiliary feed rate for use of the secondary cutting edge
Note for milling operations:
 Main feed rate for machining in the milling plane
 Auxiliary feed rate for infeed movements
For threading, drilling and milling operations, the cutting speed is
converted into rotational speed.
Coolant: Depending on the workpiece material, cutting material and
machining operation, define in the technology database whether
coolant is used. The AWG activates the appropriate coolant circuits for
the respective tool.
If you have specified that coolant is to be used, the AWG activates the
coolant circulation for the respective machining block.
Inside contours
TURN PLUS machines continuous inside contours up to the transition
from the "deepest point" to a greater diameter. The end position for
drilling, roughing and finishing operations depends on:
 Cutting limit, inside
 Overhang length, inside ULI (Processing machining parameter)
Prerequisite: The usable tool length must be sufficient for the
machining operation. If it is not, then this parameter defines the inside
machining operation. The following examples explain the principle.
Limits for internal machining operations
 Predrilling: SBI limits the drilling operation.
 Roughing: SBI or SU limit the roughing operation.
 SU = basic length of roughing cut (sbl) + overhang length, inside
(ULI)
 To avoid residual rings during the machining process, TURN PLUS
leaves an area of 5° in front of the roughing limit.
 Finishing: sbl limits the finishing operation.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
569
7.3 Machining information
Roughing limit in front of cutting limit
Example 1: The roughing limit (SU) is located in front of the cutting
limit, inside (SBI).
Abbreviations
 SBI: Cutting limit, inside
 SU: Roughing limitation (SU = sbl + ULI)
 sbl: Basic length of roughing cut ("deepest" point of inside contour)
 ULI: Overhang length, inside (machining parameter 4)
 nbl: Usable tool length (tool parameter)
570
TURN PLUS
7.3 Machining information
Roughing limit behind cutting limit
Example 2: The roughing limit (SU) is located behind the cutting limit,
inside (SBI).
Abbreviations
 SBI: Cutting limit, inside
 SU: Roughing limitation (SU = sbl + ULI)
 sbl: Basic length of roughing cut ("deepest" point of inside contour)
 ULI: Overhang length, inside (machining parameter 4)
 nbl: Usable tool length (tool parameter)
HEIDENHAIN MANUALplus 620, CNC PILOT 640
571
7.3 Machining information
Shaft machining
For shafts, TURN PLUS supports rear-face machining of outside
contours in addition to standard machining processes. This enables
shafts to be completely machined using one setup. You can select the
clamping type for the shaft machining (Shaft/chuck or Shaft/face
driver) in the V input parameter in the chucking equipment dialog.
TURN PLUS does not support retracting the tailstock and does not
check the setup used.
Precondition for shaft machining: The workpiece is clamped at
spindle and tailstock.
Danger of collision!
TURN PLUS does not monitor for collisions during
transverse machining or machining operations on the end
face.
Separation point (TR)
The separation point (TR) divides the workpiece into front and rear
area. If no separation point has been specified, TURN PLUS sets a
separation point at the transition from the largest to a smaller
diameter. Position the separation points on outside corners.
Tools for machining the
 Area on front side: Main machining direction –Z; or primarily "left"
recessing or tapping tools, etc.
 Area on rear side: Main machining direction +Z; or primarily "right"
recessing or tapping tools, etc.
Setting/changing the separation point: see "Separation point G44" on
page 222.
Protection zones for drilling and milling operations
TURN PLUS machines drilling and milling contours on transverse
surfaces (front/rear face) if:
 (Horizontal) distance to transverse surface > 5 mm, or
 Distance between chucking equipment and drilling/milling contour is
> SAR
(SAR: See user parameter).
If jaws are used for clamping the shaft at the spindle, TURN PLUS
accounts for the cutting limitation (O).
572
TURN PLUS
7.3 Machining information
Machining information
 Chucking the workpiece at the spindle: Ensure that the area,
where the blank part is chucked, is premachined. Otherwise, the
cutting limitation might adversely affect the machining strategies.
 Machining of bars: TURN PLUS does not control the bar loader
and does not move the tailstock and steady rest components. TURN
PLUS does not support workpiece adjustment between collet and
dead center during machining operations.
 Transverse machining
 Please note that the entries made in the machining sequence
apply to the complete workpiece and thus also to the transverse
machining of shaft ends.
 The AWG does not machine inside areas on the rear face. If jaws
are used for clamping the shaft at the spindle, the rear face is not
machined.
 Longitudinal machining: First the front area is machined, then the
rear area.
 Collision prevention: If machining operations are not performed
without collisions, you can do the following:
 Add a retraction of the tailstock, a positioning of the steady rest,
etc. to the program.
 Add cutting limits to the program to avoid collisions.
 Disable automatic machining in the AWG by assigning the
"Exclusion from machining" attribute or by defining a specific
machining location in the machining sequence.
 Define an oversize=0 for the workpiece blank. As a consequence,
the front area is not machined (e.g. shafts cut to length and
centered shafts).
HEIDENHAIN MANUALplus 620, CNC PILOT 640
573
7.4 Example
7.4
Example
On the basis of the production drawing, the working steps for defining
the contour of the blank and finished part, the setup procedures and
automatic working plan generation are explained.
Workpiece blank: Ø60 X 80; Material: Ck 45
 Undefined chamfers: 1x45°
 Undefined radii: 1 mm
Creating a program




Select "Program > New > New DINplus Program." The control opens
the "Save as" dialog box.
Enter a program name and press the "Save" soft key.
The control opens the "Program head (short)" dialog box.
Select a material from the fixed-word list and press the "OK" soft
key.
Workpiece blank definition



Select "ICP > Blank > Bar." TURN PLUS opens the "Bar" dialog box.
Inputs:
 Diameter X = 60 mm
 Length Z = 80 mm
 Oversize K = 2 mm
TURN PLUS displays the workpiece blank.
 Press the "Back" soft key to return to the main menu.
574
TURN PLUS
7.4 Example
Defining the basic contour

Select "ICP > Finished part (> Contour)."
 Enter start point of the contour X = 0; Z = 0 and end
point of the element X = 16

Enter Z = –25

Enter X = 35

Enter Z = –43

Enter X = 58; W = 70

Enter Z = –76

Press the "Back" soft key to go back one menu level.
Defining form elements
Chamfer at corner of threaded shank:

Select the form elements.

Select "Form > Chamfer."

Select the corner of the threaded shank.

"Chamfer" dialog box: Chamfer width = 3 mm
Rounding arcs:

Select "Form > Rounding."

Select the corners for the rounding arcs.

"Rounding" dialog box: Rounding radius = 2 mm

Select "Form > Undercut > Undercut type G."

Select the corner for the undercut.

"Undercut type DIN 76" dialog box

Select "Form > Recess > Recess standard / G22."

Select the basic element for the recess.

"Recess standard / G22" dialog box:
Undercut:
Recess:
 Inside corner (Z) = 25 mm
 Inside corner (Ki) = –8 mm
 Recess diameter = 25 mm
 Outside radius/chamfer (B) = –1 mm
HEIDENHAIN MANUALplus 620, CNC PILOT 640
575
7.4 Example
Thread:



Select "Form > Thread."
Select the basic element for the thread.
"Thread" dialog box: Select "ISO DIN 13"
 Press the "Back" soft key to return to the main menu.
Preparing the machining process, chucking
Depending on the "Zero point shift" machine parameter,
TURN PLUS automatically calculates the required zero
point shift for the workpiece and activates it with G59.
To calculate the zero point shift, TURN PLUS takes the
following values into account:
 Workpiece length Z (description of workpiece blank)
 Oversize K (description of workpiece blank)
 Edge of chuck Z (description of chucking equipment and
machining parameters)
 Edge of chuck B (description of chucking equipment and
machining parameters)



Select "Head > Chucking equipment"
Describe the chucking equipment:
 Select "AWG spindle number"
 Enter the edge of chuck
 Enter the chuck width
 Enter the cutting limitation (outside and inside)
 Enter the clamping diameter
 Enter the clamping length
 Define the clamping form
 Select "Shaft machining AWG"
TURN PLUS takes the chucking equipment and cutting limitation
into account for the program creation.
 Press the "Back" soft key to return to the main menu.
576
TURN PLUS
7.4 Example
Generating and saving a working plan
Generating a working plan


Select "TURN PLUS > AWG."
Start the AWG control graphic
Save a program




Press the "Back" soft key to return to the TURN PLUS menu.
Press the "Back" soft key to return to the Program view
Check/edit the file name and press the "Save" soft key
TURN PLUS saves the NC program
The AWG generates the work blocks according to the
machining sequence and the settings of the machining
parameters.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
577
7.5 Full-surface machining with TURN PLUS
7.5
Full-surface machining with
TURN PLUS
Rechucking the workpiece
The control uses subprograms for rechucking, which are
adapted by the machine tool builder. The functions and
sequences described below are examples—the behavior
of your machine may be different. Refer to your machine
manual.
TURN PLUS provides three full-surface machining variants:
 Rechucking the workpiece in the main spindle. Both setups are
contained in one NC program.
 Transferring the workpiece from the main spindle to the opposing
spindle (chuck part).
 Parting and picking-off the workpiece with the opposing spindle.
TURN PLUS selects the required rechucking variant on the basis of the
fixture and the machining sequence.
For every rechucking variant, a separate subprogram that
controls the rechucking sequence is defined in the user
parameters (Processing/ExpertPrograms/Expert
programs).
578
TURN PLUS
The full-surface machining sequence is defined in the chuckingequipment dialog. You also define the zero points, pick-up position and
cutting limits in this dialog.
Example of first setup for full-surface machining:
Parameters
No. of clamping H
CLAMPS 1
Spindle number AWG D
0: Main spindle
Clamp type R
0: External clamping or 1: Internal
clamping
Chuck edge Z
No entry (AWG uses the value from the
user parameters)
Chuck jaw reference B
No entry (AWG uses the value from the
user parameters)
Clamping length or free
Enter the clamping length or free length
length J
Cutting limit, outside O
Is calculated by AWG (if external
clamping is used)
Cutting limit, inside I
Is calculated by AWG (if internal
clamping is used)
Overlap K
Overlap jaw/workpiece
Chuck diameter X
Clamping diameter of workpiece blank
Chuck form Q
4: External or 5: Internal
Shaft machining V
Select the desired AWG strategy
Beispiel: Defining the first chucking equipment
Example of second setup for full-surface machining:
Parameters
No. of clamping H
CLAMPS 2
Spindle number AWG D
0: Main spindle or 3: Opposing spindle
(depending on type of rechucking)
Clamp type R
0: External clamping or 1: Internal
clamping
Chuck edge Z
No entry (AWG uses the value from the
user parameters)
Chuck jaw reference B
No entry (AWG uses the value from the
user parameters)
Clamping length or free
Enter the clamping length or free length
length J
Cutting limit, outside O
Is calculated by AWG (if external
clamping is used)
Cutting limit, inside I
Is calculated by AWG (if internal
clamping is used)
Overlap K
Overlap jaw/workpiece
Chuck diameter X
Clamping diameter of workpiece blank
Chuck form Q
4: External or 5: Internal
Shaft machining V
Select the desired AWG strategy
Beispiel: Defining the second chucking equipment
HEIDENHAIN MANUALplus 620, CNC PILOT 640
...
CLAMPS 1
H0 D0 R0 J100 K15 X120 Q4 V0
...
...
CLAMPS 2
H0 D3 R1 J15 K-15 X68 Q4 V0
...
579
7.5 Full-surface machining with TURN PLUS
Defining the chucking equipment for full-surface
machining
7.5 Full-surface machining with TURN PLUS
Automatic program creation for full-surface
machining
During automatic program creation (AWG) the machining steps for the
first setup are created first. Then AWG opens a dialog window that
requests the parameters for rechucking.
Default values that were calculated by AWG from the defined
workpiece contour are already entered in the parameters in the dialog
window. You can use or change these values. After you have
confirmed the values, AWG generates the machining sequence for
the second setup.
In the user parameters the machine manufacturer defines
the input parameters to be displayed in the dialog
windows during rechucking.
You can also include further input parameters in the dialog
windows. To do this, select the required parameters list
(Processing/ExpertPrograms/Parameter lists for expert
programs) in the user parameters. In the desired
parameter enter a default value that is assigned to this
parameter in the dialog window. Enter 9999999 to display
the parameter without a default value.
Rechucking the workpiece in the main spindle
The subprogram for "rechucking in the main spindle" is defined in the
user parameter Parameter list – manual rechucking (standard
program: Rechuck_manual.ncs).
At the end of the machining sequence, define a machining step with
the rechucking main machining operation and the full-surface
machining submachining operation.
In parameter D of the chucking equipment description, select the main
spindle for both pieces of chucking equipment.
Beispiel: Defining the chucking equipment
...
CLAMPS 1
H0 D0 R0 J80 K15 X120 Q4 V0
CLAMPS 2
H0 D0 R1 J15 K-15 X68 Q4 V0
...
Transferring the workpiece from the main
spindle to the opposing spindle
The subprogram for "transferring the workpiece from the main spindle
to the opposing spindle" is defined in the user parameter Parameter
list – complete rechucking (standard program:
Rechuck_complete.ncs).
Beispiel: Defining the chucking equipment
...
CLAMPS 1
At the end of the machining sequence, define a machining step with
the rechucking main machining operation and the full-surface
machining submachining operation.
H0 D0 R0 J80 K15 X120 Q4 V0
In parameter D of the chucking equipment description, select the main
spindle for the first chucking equipment and the opposing spindle for
the second chucking equipment.
H0 D3 R1 J15 K-15 X68 Q4 V0
580
CLAMPS 2
...
TURN PLUS
7.5 Full-surface machining with TURN PLUS
Parting and picking-off the workpiece with the
opposing spindle
The subprogram for "parting and picking-off with the opposing spindle"
is defined in the user parameter Parameter list – rechucking,
parting (standard program: Rechuck_complete.ncs).
At the end of the machining sequence, define a machining step with
the parting main machining operation and the full-surface
machining submachining operation.
In parameter D of the chucking equipment description, select the main
spindle for the first chucking equipment and the opposing spindle for
the second chucking equipment.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
Beispiel: Defining the chucking equipment
...
CLAMPS 1
H0 D0 R0 J100 K15 X120 Q4 V0
CLAMPS 2
H0 D3 R1 J15 K-15 X68 Q4 V0
...
581
582
TURN PLUS
7.5 Full-surface machining with TURN PLUS
B axis
8.1 Fundamentals
8.1 Fundamentals
Tilted working plane
The machine tool builder determines the scope of function
and behavior of the B axis. The machine manual provides
further information.
Tilted working plane
The B axis makes it possible to drill, bore and mill in oblique planes. To
make programming easy, the coordinate system is tilted in such a way
that you can define the drilling patterns and milling contours in the YZ
plane. The actual drilling or milling operation is then performed in the
tilted plane (see „Tilting the working plane G16” on page 522).
The separation of contour description and machining also applies to
machining operations in tilted planes. Contour regeneration is not
available.
Contours in tilted planes are identified by the section code
LATERAL_Y (see „LATERAL_Y section” on page 52).
The control supports NC program creation with the B axis in DIN PLUS
and smart.Turn.
The graphical simulation shows the machining operation in a tilted
working plane in the familiar lathe and front windows, as well as in the
"side view (YZ)."
If you are using a tool with an angled tool holder you can
also use the tilted working plane without the B axis. Define
the angle for the tool holder as angular offset RW in the tool
description.
584
B axis
BW 90
In this way, you need fewer tools and fewer tool changes.
Tool data: All tools are described in the tool database by specifying
the X, Z and Y dimensions as well as the compensation values. These
dimensions are referenced to the tilt angle B=0° (reference position).
8.1 Fundamentals
Tools for the B axis
Another advantage of the B axis is that it allows flexible use of the
tools during turning operations. By tilting the B axis and rotating the
tool you can bring it into positions that enable you to use one and the
same tool to machine in the longitudinal and transverse (or radial and
axial) directions on the main and opposing spindles.
BW 180
CW 0
BW 0
BW 90
Another parameter that is maintained in the tool database is the
position angle CW. It defines the working positions of tools that are
not driven tools (turning tools).
The tilt angle of the B axis is not maintained with the tool data. This
angle needs to be defined in the tool call or when inserting the tool.
CW 1
Tool orientation and position display: For turning tools, the position
of the tool tip is calculated based on the orientation of the cutting
edge.
The control calculates the tool orientation of lathe tools by means of
the tool angle and point angle.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
585
8.1 Fundamentals
Multipoint tools for the B axis
If several tools are mounted on a tool holder, this is referred to as a
"multipoint tool." Each cutting edge (tool) of a multipoint tool is
assigned a separate ID number and description.
The position angle, which is identified by "CW" in the figure, is
included in the tool data.When a cutting edge (tool) of a multipoint tool
is activated, the CNC PILOT will rotate the multipoint tool into the
correct position. The position is determined from the position angle, to
which the offset position angle from the tool change routine is added.
This allows inserting the tool either in the "normal" attitude or "upside
down."
CW240
CW0
The photo shows a multipoint tool with three cutting edges.
CW120
586
B axis
8.2 Compensation with the B axis
8.2 Compensation with the B axis
Compensation during program run
Tool compensation: Enter the compensation values determined in
the tool compensation form. Also define further functions that were
active while machining the measured surface:
 Tilt angle of the B axis BW
 Position angle of the tool CW
 Kinematics KM
 Plane G16
The control converts the measured data into dimensions referenced to
the position B=0 and saves them in the tool database.

Select the Tool/Add correct. soft key during program
run.

The control opens "Set the tool compensation" in the
dialog box.

Enter new values.

Press the Save soft key.
In the "T" box (machine display), the control indicates the
compensation values referenced to the current B axis angle and the
tool position angle.
 The control saves the tool compensation data in the tool
database, together with the other tool data.
 If the B axis is tilted, the control takes the tool
compensation data into account when calculating the
tool tip position.
Additive compensation values are independent of the tool data.
The compensation values are effective in the X, Y and Z directions.
Tilting the B axis has no influence on additive compensation values.
HEIDENHAIN MANUALplus 620, CNC PILOT 640
587
8.3 Simulation
8.3 Simulation
Simulation of the tilted plane
3-D view: The simulation correctly displays tilted Y planes as well as
elements referenced to them (such as pockets, holes, patterns, etc.).
Contour graphics: The simulation displays the YZ view of the
workpiece and the contours of the tilted planes in the side view. To
represent the drilling patterns and milling contours perpendicularly to
the tilted plane, i.e. without distortion, the simulation ignores the
rotation of the coordinate system and a shift within the rotated
coordinate system.
Beispiel: "Contour in tilted plane"
...
FINISHED
N2 G0 X0 Z0
N3 G1 X50
N4 G1 Z–50
With contour graphics for tilted planes, please note the following:
N5 G1 X0
 The parameter "K" of G16 or LATERAL_Y defines the "start" of the
drilling pattern or milling contour in the Z direction.
 The drilling patterns and milling contours are drawn perpendicularly
to the tilted plane. This results in a "shift" relative to the turning
contour.
N6 G1 Z0
Milling, drilling and boring operations: When you use the side
view to display the tool paths in the tilted plane, the same rules apply
as for the contour graphics.
LATERAL_Y X50 C0 B20 I25 K-20 H1
LATERAL_Y X50 C0 B80 I25 K-10 H0
N7 G386 Z0 Ki10 B–30 X50 C0 [Single
surface]
N8 G384 Z–10 Y10 X50 R10 P5 [Full circle]
...
When working in tilted planes, the front window shows the "outline"
of the tool. The tool width is simulated true to scale. In this way, you
can check the overlap of milling paths. The tool paths are also
represented true to scale (in perspective view) as line graphics.
In all "additional windows," the simulation shows the tool and the
cutting path when the tool is perpendicular to the relevant plane. A
tolerance of +/– 5° is taken into account. When the tool is not
perpendicular to the plane, it is represented as a "light dot" and the tool
path is depicted as a line.
588
B axis
8.3 Simulation
Displaying the coordinate system
The simulation can show the shifted/rotated coordinate system in the
"lathe window," if required. To use this feature, you need to stop the
simulation.

Press the Plus/Minus key. The simulation displays the
current coordinate system.
The coordinate system disappears when the next command is
simulated or when you press the Plus/Minus key once again.
Position display with the B and Y axes
The following boxes of the display cannot be edited:
 N: Block number of the NC source block
 X, Z, C: Position values (actual values)
The other boxes can be set with the Split-Screen Layout key (three
arrows arranged in a circle):
 Default settings (values of the selected slide):
 Y: Position value (actual value)
 T: Tool data with turret pocket (in "(..)") and ID number
 B axis settings:
 B: Tilt angle of the B axis
 G16/B: Angle of the tilted plane
HEIDENHAIN MANUALplus 620, CNC PILOT 640
589
590
B axis
8.3 Simulation
Overview of units
9.1 Units—"Turning" group
9.1 Units—"Turning" group
"Roughing" group
Unit
Description
Page
G810_ICP
G810 Longitudinal in ICP
Page 67
Roughing an ICP contour longitudinally
G820_ICP
G820 Transverse in ICP
Page 68
Roughing an ICP contour transversely
G830_ICP
G830 Contour parallel in ICP
Page 69
Roughing parallel to the contour in ICP
G835_ICP
G835 Bidirectional in ICP
Page 70
Roughing an ICP contour in two directions
G810_G80
G810 Longitudinal, direct
Page 71
Longitudinal roughing with direct contour input
G820_G80
G820 Transverse, direct
Page 72
Transverse roughing with direct contour input
"Finishing" group
Unit
Description
Page
G890_ICP
G890 Contouring in ICP
Page 118
Finishing an ICP contour
G890_G80_L
G890 Contouring, direct longitdnl.
Page 120
Longitudinal finishing with direct contour input
G890_G80_P
G890 Contouring, direct transverse
Page 121
Transverse finishing with direct contour input
G85x_DIN_E_F_G
G890 Relief, type E, F, DIN76
Page 122
Finishing the undercuts according to DIN509 type E and F and the thread
undercut DIN76
592
Overview of units
9.1 Units—"Turning" group
"Recessing" group
Unit
Description
Page
G860_ICP
G860 Contour recess in ICP
Page 73
Recessing an ICP contour
G869_ICP
G869 Recess turning in ICP
Page 74
Recess turning an ICP contour
G860_G80
G860 Contour recess, direct
Page 75
Contour recessing with direct contour input
G869_G80
G869 Recess turning, direct
Page 76
Recess turning with direct contour input
G859_Cut_off
G859 Parting
Page 77
Parting a bar with direct position input
G85x_Cut_H_K_U
G85X Undercutting (H, K, U)
Page 78
Make undercuts of type H, K and U
"Thread" group
Unit
Description
Page
G32_MAN
G32 Single thread
Page 127
Thread with direct contour definition
G31_ICP
G31 ICP thread
Page 128
Thread on any desired ICP contour
G352_API
G352 API thread
Page 130
API thread with direct contour definition
G32_KEG
G32 Tapered thread
Page 131
Tapered thread with direct contour definition
HEIDENHAIN MANUALplus 620, CNC PILOT 640
593
9.2 Units—"Drilling" group
9.2 Units—"Drilling" group
"Centric drilling" group
Unit
Description
Page
G74_Zentr
G74 Centric drilling
Page 80
Drilling and pecking with X=0
G73_Zentr
G73 Centric tapping
Page 82
Tapping with X=0
"ICP drilling, C axis" group
Unit
Description
Page
G74_ICP_C
G74 ICP drilling, C axis
Page 102
Drilling and pecking with ICP pattern
G73_ICP_C
G73 ICP tapping, C axis
Page 104
Tapping with ICP pattern
G72_ICP_C
G72 ICP boring, countersinking in C axis
Page 105
Tapping with ICP pattern
"C-axis face drilling" group
Unit
Description
Page
G74_Bohr_Stirn_C
G74 Single hole
Page 84
Drilling and pecking a single hole
G74_Lin_Stirn_C
G74 Linear pattern drilling
Page 86
Drilling and pecking a linear hole pattern
G74_Cir_Stirn_C
G74 Circ. pattern drilling
Page 88
Drilling and pecking a circular hole pattern
G73_Gew_Stirn_C
G73 Tapping
Page 90
Tapping a single hole
G73_Lin_Stirn_C
G73 Thread, linear pattern
Page 91
Tapping a linear hole pattern
G73_Cir_Stirn_C
G73 Thread, circular pattern
Page 92
Tapping a circular hole pattern
594
Overview of units
9.2 Units—"Drilling" group
"C-axis lateral surface drilling" group
Unit
Description
Page
G74_Bohr_Mant_C
G74 Single hole
Page 93
Drilling and pecking a single hole
G74_Lin_Mant_C
G74 Linear pattern drilling
Page 95
Drilling and pecking a linear hole pattern
G74_Cir_Mant_C
G74 Circ. pattern drilling
Page 97
Drilling and pecking a circular hole pattern
G73_Gew_Mant_C
G73 Tapping
Page 99
Tapping a single hole
G73_Lin_Mant_C
G73 Thread, linear pattern
Page 100
Tapping a linear hole pattern
G73_Cir_Mant_C
G73 Thread, circular pattern
Page 101
Tapping a circular hole pattern
HEIDENHAIN MANUALplus 620, CNC PILOT 640
595
9.3 Units—"Predrilling in C axis" group
9.3 Units—"Predrilling in C axis"
group
"Predrilling in C-axis, face" group
Unit
Description
Page
DRILL_STI_KON_C
G840 Predrill face, contour milling, figures
Page 106
Determine the predrilling position and machine a hole
DRILL_STI_840_C
G840 Predrill face, ICP contour milling
Page 108
Determine the predrilling position and machine a hole
DRILL_STI_TASC
G845 Predrill face, pocket milling, figures
Page 109
Determine the predrilling position and machine a hole
DRILL_STI_845_C
G845 Predrill face, ICP pocket milling
Page 111
Determine the predrilling position and machine a hole
"Predrilling in C-axis, lateral surface" group
Unit
Description
Page
DRILL_MAN_KON_C
G840 Predrill latrl., contour milling, figures
Page 112
Determine the predrilling position and machine a hole
DRILL_MAN_840_C
G840 Predrill lateral surf., ICP contour milling
Page 114
Determine the predrilling position and machine a hole
DRILL_MAN_TAS_C
G845 Predrill lateral surf., pocket milling, figures
Page 115
Determine the predrilling position and machine a hole
DRILL_MAN_845_C
G845 Predrill lateral surf., ICP pocket milling
Page 117
Determine the predrilling position and machine a hole
596
Overview of units
9.4 Units—"Milling in C axis" group
9.4 Units—"Milling in C
axis" group
"Milling in C-axis, face" group
Unit
Description
Page
G791_Nut_Stirn_C
G791 Linear slot
Page 133
Milling a linear slot
G791_Lin_Stirn_C
G791 Linear slot pattern
Page 134
Milling of linear slots in a linear pattern
G791_Cir_Stirn_C
G791 Circular slot pattern
Page 135
Milling of linear slots in a circular pattern
G797_STIRNFR_C
G797 Face milling
Page 136
Milling various figures as islands
G797_ICP
G797 Face milling ICP
Page 137
Milling closed contours as islands
G799_GewindeFR_C
G799 Thread milling
Page 138
Inside thread milling in a single hole
G840_FIG_STIRN_C
G840 Contour milling, figures
Page 139
Milling figures inside, outside and on the contour
G84X_FIG_STIRN_C
G84x Pocket milling, figures
Page 142
Roughing out closed figures, inside
G801_GRA_STIRN_C
G801 Engraving
Page 145
Engraving characters strings on the face
"ICP milling in C axis, face" group
Unit
Description
Page
G840_Kon_C_STIRN
G840 Contour milling, ICP
Page 141
Machining ICP contours on the face inside, outside and on the contour
G845_TAS_C_STIRN
G845 Pocket milling, ICP
Page 144
Inside rough-out of closed ICP contours on the face
G840_ENT_C_STIRN
G840 Deburring
Page 146
Deburring ICP contours on the face
HEIDENHAIN MANUALplus 620, CNC PILOT 640
597
9.4 Units—"Milling in C axis" group
"C-axis lateral surface milling" group
Unit
Description
Page
G792_NUT_MANT_C
G792 Linear slot
Page 147
Milling a linear slot
G792_LIN_MANT_C
G792 Linear slot pattern
Page 148
Milling of linear slots in a linear pattern
G792_CIR_MANT_C
G792 Circular slot pattern
Page 149
Milling of linear slots in a circular pattern
G798_Wendelnut_C
G798 Helical slot milling
Page 150
Milling a thread-shaped helical slot
G840_FIG_MANT_C
G840 Contour milling, figures
Page 151
Milling figures inside, outside and on the contour
G84x_FIG_MANT_C
G84x Pocket milling, figures
Page 154
Roughing out closed figures, inside
G802_GRA_MANT_C
G802 Engraving
Page 157
Engraving characters strings on the lateral surface
"ICP milling in C axis, lateral surface" group
Unit
Description
Page
G840_Kon_C_Mant
G840 Contour milling, ICP
Page 153
Machining ICP contours on the lateral surface inside, outside and on the contour
G845_TAS_C_MANT
G845 Pocket milling, ICP
Page 156
Inside rough-out of closed ICP contours on the lateral surface
G840_ENT_C_MANT
G840 Deburring
Page 158
Deburring ICP contours on the lateral surface
598
Overview of units
9.5 Units—"Drilling, predrilling in Y axis" group
9.5 Units—"Drilling, predrilling in Y
axis" group
"ICP drilling, Y axis" group
Unit
Description
Page
G74_ICP_Y
G74 ICP drilling, Y axis
Page 168
Drilling and pecking with ICP pattern
G73_ICP_Y
G73 ICP tapping, Y axis
Page 169
Tapping with ICP pattern
G72_ICP_Y
G72 ICP boring, countersinking in Y axis
Page 170
Tapping with ICP pattern
"Predrilling in Y axis" group
Unit
Description
Page
DRILL_STI_840_Y
G840 ICP predrilling, contour milling in XY plane
Page 171
Determine the predrilling position and machine a hole
DRILL_STI_845_Y
G845 ICP predrilling, pocket milling in XY plane
Page 172
Determine the predrilling position and machine a hole
DRILL_MAN_840_Y
G840 ICP predrilling, contour milling in YZ plane
Page 173
Determine the predrilling position and machine a hole
DRILL_MAN_845_Y
G845 ICP predrilling, pocket milling in YZ plane
Page 174
Determine the predrilling position and machine a hole
HEIDENHAIN MANUALplus 620, CNC PILOT 640
599
9.6 Units—"Milling in Y axis" group
9.6 Units—"Milling in Y axis" group
"Milling in front face" group (XY plane)
Unit
Description
Page
G840_Kon_Y_Stirn
G840 Contour milling
Page 175
Machining contours in the XY plane inside, outside and on the contour
G845_Tas_Y_Stirn
G845 Pocket milling
Page 176
Inside rough-out of closed contours in the XY plane
G840_ENT_Y_STIRN
G840 Deburring
Page 180
Deburring contours in the XY plane
G801_GRA_STIRN_C
G841 Single surface
Page 177
Milling a single surface (flat) in the XY plane
G840_Kon_C_STIRN
G843 Centric polygon
Page 178
Milling a centric polygon in the XY plane
G803_GRA_Y_STIRN
G803 Engraving
Page 179
Engraving character strings in the XY plane
G800_GEW_Y_STIRN
G800 Thread milling
Page 181
Milling a thread in an existing hole in the XY plane
600
Overview of units
9.6 Units—"Milling in Y axis" group
"Milling in lateral surface" group (YZ plane)
Unit
Description
Page
G840_Kon_Y_Mant
G840 Contour milling
Page 182
Machining contours in the YZ plane inside, outside and on the contour
G845_Tas_Y_Mant
G845 Pocket milling
Page 183
Inside rough-out of closed contours in the YZ plane
G840_ENT_Y_MANT
G840 Deburring
Page 187
Deburring contours in the YZ plane
G801_GRA_STIRN_C
G841 Single surface
Page 184
Milling a single surface (flat) in the YZ plane
G840_Kon_C_STIRN
G843 Centric polygon
Page 185
Milling a centric polygon in the YZ plane
G804_GRA_Y_MANT
G803 Engraving
Page 186
Engraving character strings in the YZ plane
G806_GEW_Y_MANT
G800 Thread milling
Page 188
Milling a thread in an existing hole in the YZ plane
HEIDENHAIN MANUALplus 620, CNC PILOT 640
601
9.7 Units—"Special units" group
9.7 Units—"Special units" group
Unit
Description
Page
START
Program beginning (START)
Page 159
For functions required at the beginning of the program
C_AXIS_ON
C axis on
Page 161
Activate C-axis interpolation
C_AXIS_OFF
C axis off
Page 161
Deactivate C-axis interpolation
SUBPROG
Subprogram call
Page 162
Calling any desired subprogram
REPEAT
Process logic—repetition
Page 163
Describing a WHILE loop to repeat parts of the program
END
Program end (END)
Page 164
For functions required at the end of the program
602
Overview of units
Overview of G codes
10.1 Section codes
10.1 Section codes
Program section codes
Program head
Program section codes
Y-axis contours
PROGRAMMKOPF / HEADER
Page 48
STIRN_Y / FACE_Y
Page 51
REVOLVER / TURRET
Page 50
RUECKSEITE_Y / REAR_Y
Page 51
SPANNMITTEL / CLAMPS
Page 49
MANTEL_Y / LATERAL_Y
Page 52
Contour definition
Workpiece machining
ROHTEIL / BLANK
Page 50
BEARBEITUNG / MACHINING
Page 53
HILFSROHTEIL / AUXIL_BLANK
Page 50
ENDE / END
Page 53
FERTIGTEIL / FINISHED
Page 50
HILFSKONTUR / AUXIL_CONTOUR
Page 50
Subprograms
UNTERPROGRAMM / SUBPROGRAM Page 53
C-axis contours
604
RETURN
Page 53
Others
STIRN / FACE_C
Page 51
RUECKSEITE / REAR_C
Page 51
CONST
Page 54
MANTEL / LATERAL_C
Page 51
VAR
Page 54
Overview of G codes
G commands for turning contours
Turning contour
Workpiece-blank definition
Turning contour
Contour form elements
G20-Geo
Chuck part, cylinder/tube
Page 200
G22-Geo
Recess (standard)
Page 207
G21-Geo
Cast part
Page 200
G23-Geo
Recess/relief turn
Page 209
G24-Geo
Thread with undercut
Page 211
Basic contour elements
G0-Geo
Starting point of contour
Page 201
G25-Geo
Undercut contour
Page 212
G1-Geo
Line segment
Page 202
G34-Geo
Thread (standard)
Page 216
G2-Geo
Circular arc cw with incremental
center dimensioning
Page 204
G37-Geo
Thread (general)
Page 217
G3-Geo
Circular arc ccw with incremental
center dimensioning
Page 204
G49-Geo
Bore hole at turning center
Page 219
G12-Geo
Circular arc cw with absolute center Page 205
dimensioning
Help commands for contour definition
G13-Geo
Circular arc ccw with absolute
center dimensioning
Overview: Attributes for contour description
Page 220
G38-Geo
Feed rate reduction
Page 220
G44
Separation point
Page 222
G52-Geo
Oversize
Page 222
G95-Geo
Feed per revolution
Page 223
Page 205
G149-Geo Additive compensation
HEIDENHAIN MANUALplus 620, CNC PILOT 640
Page 223
605
10.2 Overview of G commands in the CONTOUR section
10.2 Overview of G commands in
the CONTOUR section
10.2 Overview of G commands in the CONTOUR section
G commands for C-axis contours
C-axis contour
Overlapping contours
G308-Geo Beginning of pocket/island
C-axis contour
Overlapping contours
Page 224
Front and rear face contours
G309-Geo End of pocket/island
Page 224
Lateral surface contours
G100-Geo Starting point of contour, face
Page 230
G110-Geo Starting point of lateral surface
contour
Page 239
G101-Geo Line segment, face
Page 231
G111-Geo Line segment, lateral surface
Page 240
G102-Geo Arc cw, face
Page 232
G112-Geo Arc cw, lateral surface
Page 241
G103-Geo Arc ccw, face
Page 232
G113-Geo Arc ccw, lateral surface
Page 241
G300-Geo Bore hole, face
Page 233
G310-Geo Bore hole on lateral surface
Page 242
G301-Geo Linear slot, face
Page 234
G311-Geo Linear slot on lateral surface
Page 243
G302-Geo Circular slot cw, face
Page 234
G312-Geo Circular slot cw, lateral surface
Page 243
G303-Geo Circular slot ccw, face
Page 234
G313-Geo Circular slot ccw, lateral surface
Page 243
G304-Geo Full circle, face
Page 235
G314-Geo Full circle, lateral surface
Page 244
G305-Geo Rectangle, face
Page 235
G315-Geo Rectangle, lateral surface
Page 244
G307-Geo Polygon, face
Page 236
G317-Geo Polygon, lateral surface
Page 245
G401-Geo Pattern linear, face
Page 237
G411-Geo Pattern linear, lateral surface
Page 246
G402-Geo Pattern circular, face
Page 238
G412-Geo Pattern circular, lateral surface
Page 247
G commands for Y-axis contours
Y-axis contour
XY plane
Y-axis contour
YZ plane
G170-Geo Starting point of contour in XY
plane
Page 504
G180-Geo Starting point of contour in YZ
plane
Page 513
G171-Geo Line segment in XY plane
Page 504
G181-Geo Line segment in YZ plane
Page 513
G172-Geo Arc cw in XY plane
Page 505
G182-Geo Arc cw in YZ plane
Page 514
G173-Geo Arc ccw in XY plane
Page 505
G183-Geo Arc ccw in YZ plane
Page 514
G370-Geo Hole in XY plane
Page 506
G380-Geo Hole in YZ plane
Page 515
G371-Geo Linear slot in XY plane
Page 507
G381-Geo Linear slot in YZ plane
Page 515
G372-Geo Circular slot cw in XY plane
Page 508
G382-Geo Circular slot cw in YZ plane
Page 516
G373-Geo Circular slot ccw in XY plane
Page 508
G383-Geo Circular slot ccw in YZ plane
Page 516
G374-Geo Full circle in XY plane
Page 508
G384-Geo Full circle in YZ plane
Page 516
G375-Geo Rectangle in XY plane
Page 509
G385-Geo Rectangle in YZ plane
Page 517
G377-Geo Polygon in XY plane
Page 509
G387-Geo Polygon in YZ plane
Page 517
G471-Geo Pattern linear in XY plane
Page 510
G481-Geo Pattern linear in YZ plane
Page 518
G472-Geo Pattern circular in XY plane
Page 511
G482-Geo Pattern circular in YZ plane
Page 519
G376-Geo Single surface in XY plane
Page 512
G386-Geo Single surface in XY plane
Page 520
G477-Geo Centric polygon in XY plane
Page 512
G487-Geo Centric polygon in XY plane
Page 520
606
Overview of G codes
G commands for turning
Turning—Basic functions
Tool positioning without machining
Turning—Basic functions
Zero point shifts
G0
Positioning at rapid traverse
Page 248
Overview: Zero point shifts
Page 259
G14
Move to the tool change position
Page 249
G51
Zero point shift
Page 260
G140
Define the tool change position
Page 249
G53/
G54/
G55
Zero point offsets
Page 261
G701
Rapid traverse to machine
coordinates
Page 248
G56
Additive zero-point shift
Page 261
G59
Absolute zero point shift
Page 262
Simple linear and circular movements
G1
Linear movement
Page 250
G152
Zero point shift, C axis
Page 339
G2
Circular movement cw with
incremental center dimensioning
Page 251
G920
Deactivate zero point shifts
Page 384
G3
Circular movement ccw with
incremental center dimensioning
Page 251
G921
Deactivate zero point shift, tool
dimensions
Page 384
G12
Circular movement cw with absolute Page 252
center dimensioning
G980
Activate zero point shift
Page 387
G13
Circular movement ccw with
absolute center dimensioning
G981
Activate zero point shift, tool
dimensions
Page 387
Page 252
Feed rate and spindle speed
Safety clearances
Gx26
Speed limit *
Page 253
G47
Set safety clearances
Page 265
G64
Interrupted feed
Page 254
G147
Safety clearance (milling)
Page 265
G48
Reduce rapid traverse
Page 253
Tool-tip radius compensation (TRC/MCRC)
Gx93
Feed per tooth *
Page 254
G40
Switch off TRC/MCRC
Page 257
G94
Feed per minute
Page 255
G41
TRC/MCRC, left
Page 258
Gx95
Feed per revolution
Page 255
G42
TRC/MCRC, right
Page 258
Gx96
Constant surface speed
Page 256
Tools, types of compensation
Gx97
Speed
Page 256
T
Tool change
Page 266
G148
(Changing the) cutter compensation
Page 267
Oversizes
G50
Switch off oversize
Page 263
G149
Additive compensation
Page 268
G52
Switch off oversize
Page 263
G150
Compensate right tool tip
Page 269
G57
Paraxial oversize
Page 263
G151
Compensate left tool tip
Page 269
G58
Contour-parallel oversize
Page 264
HEIDENHAIN MANUALplus 620, CNC PILOT 640
607
10.3 Overview of G commands in the MACHINING section
10.3 Overview of G commands in
the MACHINING section
10.3 Overview of G commands in the MACHINING section
Cycles for turning
Turning—Cycles
Simple turning cycles
Turning—Cycles
Contour-based turning cycles
G80
Cycle end / simple contours
Page 294
G740
Contour repeat cycle
Page 285
G81
Simple longitudinal roughing
Page 434
G741
Contour repeat cycle
Page 285
G82
Simple face roughing
Page 435
G810
Longitudinal roughing cycle
Page 272
G83
Contour repeat cycle
Page 436
G820
Face roughing cycle
Page 275
G86
Simple recessing cycle
Page 437
G830
Contour-parallel roughing cycle
Page 278
G87
Transition radii
Page 438
G835
Contour-parallel with neutral tool
Page 281
G88
Chamfers
Page 438
G860
Universal recessing cycle
Page 283
G869
Recess turning cycle
Page 286
Drilling cycles
G36
Tapping
Page 330
G870
Simple recessing cycle G22
Page 289
G71
Simple drilling cycle
Page 325
G890
Finishing cycle
Page 290
G72
Boring, countersinking, etc.
Page 327
Thread cycles
G73
Tapping cycle
Page 328
G31
Thread cycle
Page 303
G74
Deep-hole drilling cycle
Page 331
G32
Single thread cycle
Page 307
G33
Single thread cut (Thread single path) Page 309
Undercuts
G25
Undercut contour
Page 212
G35
Metric ISO thread
G85
Undercut
Page 316
G350
Simple longitudinal thread
G851
Undercut DIN 509 E, direct
Page 318
G351
Simple longitudinal multi-start thread
G852
Undercut DIN 509 F, direct
Page 319
G352
Tapered API thread
G853
Undercut DIN 76 thread, direct
Page 320
G36
Tapping
Page 330
G856
Undercut type U, direct
Page 321
G38
Metric ISO thread
Page 314
G857
Undercut type H, direct
Page 322
Parting
G858
Undercut type K, direct
Page 323
G859
Parting cycle
Page 315
608
Page 311
Page 312
Overview of G codes
C-axis machining
C axis
C-axis machining
G120
Reference diameter, lateral-surface
machining
Page 339
G152
Zero point shift, C axis
Page 339
G153
Standardize C axis
Page 340
Single path—Front/rear face machining
Single path—Lateral-surface machining
G100
Rapid traverse, face
Page 341
G110
Rapid traverse, lateral surface
Page 345
G101
Linear path, face
Page 342
G111
Linear path, lateral surface
Page 346
G102
Circular path cw, face
Page 343
G112
Circular path cw, lateral surface
Page 347
G103
Circular path ccw, face
Page 343
G113
Circular path ccw, lateral surface
Page 347
Figures—Front/rear face machining
Figures—Lateral-surface machining
G301
Linear slot, face
Page 295
G311
Linear slot on lateral surface
Page 297
G302
Circular slot cw, face
Page 295
G312
Circular slot cw, lateral surface
Page 298
G303
Circular slot ccw, face
Page 295
G313
Circular slot ccw, lateral surface
Page 298
G304
Full circle, face
Page 296
G314
Full circle, lateral surface
Page 298
G305
Rectangle, face
Page 296
G315
Rectangle, lateral surface
Page 299
G307
Polygon, face
Page 296
G317
Polygon, lateral surface
Page 299
Milling cycles, face
Milling cycles, lateral surface
G791
Linear slot, face
Page 349
G792
Linear slot, lateral surface
Page 350
G793
Contour milling, direct
Page 351
G794
Contour milling, direct
Page 353
G797
Area milling (face milling)
Page 355
G798
Helical slot milling
Page 357
G799
Thread milling
Predrilling cycles
Contour and pocket milling cycles
G840
Predrilling, contour milling
Page 359
G840
Contour milling
Page 361
G845
Predrilling, pocket milling
Page 369
G840
Deburring
Page 365
G845
Pocket milling
Page 370
Pocket milling, finishing
Page 374
Engraving cycles
G801
Engraving, face
Page 378
G846
G802
Engraving, lateral surface
Page 379
Engraving cycles
Pattern
G743
Pattern linear, face
G745
Pattern circular, face
G744
Pattern linear, lateral surface
G746
Pattern circular, lateral surface
HEIDENHAIN MANUALplus 620, CNC PILOT 640
G801
Engraving, face
Page 378
G802
Engraving, lateral surface
Page 379
Character set for engraving
Page 376
609
10.3 Overview of G commands in the MACHINING section
C-axis machining
10.3 Overview of G commands in the MACHINING section
Y-axis machining
Y-axis machining
Working planes
Y-axis machining
Milling cycles
G17
XY plane
Page 521
G841
Area milling, roughing
Page 527
G18
XZ plane (turning view)
Page 521
G842
Area milling, finishing
Page 528
G19
YZ plane
Page 521
G843
Centric polygon milling, roughing
Page 529
G844
Centric polygon milling, finishing
Page 530
Tool positioning without machining
G0
Positioning at rapid traverse
Page 523
G845
Predrilling, pocket milling
Page 532
G14
Move to the tool change position
Page 523
G845
Pocket milling, roughing
Page 533
G701
Rapid traverse to machine
coordinates
Page 523
G846
Pocket milling, finishing
Page 537
G800
Thread milling in XY plane
Page 541
Simple linear and circular movements
G1
Linear movement
Page 524
G806
Thread milling in YZ plane
Page 542
G2
Circular movement cw with
incremental center dimensioning
Page 525
G808
Hobbing
Page 543
G3
Circular movement ccw with
incremental center dimensioning
Page 525
Engraving cycles
G12
Circular movement cw with absolute Page 526
center dimensioning
G803
Engraving in XY plane
Page 539
G13
Circular movement ccw with
absolute center dimensioning
G804
Engraving in YZ plane
Page 540
Character set for engraving
Page 376
Page 526
Variable programming, program branches
Variable programming, program branches
Programming with variables
Variable programming, program branches
Data input and data output
# variables
Variable types
Page 408
INPUT
Input (# variables)
Page 405
PARA
Read configuration data
Page 418
WINDOW
Open output window (#
variables)
Page 405
CONST
Constant definition
Page 421
PRINT
Output (# variables)
Page 406
VAR
Variable definition
Page 420
Program branches, program repeats
Subprograms
Subprogram call
610
Page 427
IF..THEN..
Program branching
Page 422
WHILE..
Program repeat
Page 424
SWITCH..
Program branching
Page 425
Overview of G codes
10.3 Overview of G commands in the MACHINING section
Other G codes
Other G codes
G4
Dwell time
Page 381
Other G codes
G909 Interpreter stop
Page 383
G7
G8
Precision stop ON
Page 381
G910
Switching measurement on/off
Page 497
Precision stop OFF
Page 382
G911
Activate measuring path monitoring Page 498
G9
Precision stop (blockwise)
Page 382
G912
Actual position capture
Page 498
G30
Converting and mirroring
Page 389
G913
End in-process measurement
Page 498
G44
Separation point
Page 222
G914
Deactivate measuring path
monitoring
Page 498
G60
Deactivate protection zone
Page 382
G916
Traversing to a fixed stop
Page 394
G65
Display chucking equipment
Page 381
G919
Spindle override 100 %
Page 383
G67
Load blank-part contour (graphics)
Page 381
G920
Deactivate zero point shift
Page 384
G99
Transformations of contours
Page 391
G921
Deactivate zero point shift, tool
dimensions
Page 384
G702
Storing/loading contour follow-up
Page 380
G922
Tool end position
Page 384
G703
Contour follow-up ON/OFF
Page 380
G923
Handwheel offset in thread
Page 125
G720
Spindle synchronization
Page 392
G924
Fluctuating speed
Page 384
G725
Eccentric turning
Page 399
G925
Force reduction
Page 397
G726
Transition to eccentric
Page 401
G927
Convert tool lengths
Page 385
G727
Eccentric X
Page 403
G930
Sleeve monitoring
Page 398
G901
Actual values in variables
Page 382
G940
Automatically convert variables
Page 385
G902
Zero point shift in variables
Page 382
G980
Activate zero point shift
Page 387
G903
Lag error in variables
Page 382
G981
Activate zero point shift, tool
dimensions
Page 387
G904
Read interpolator information
Page 383
G995
Monitoring zone
Page 388
G905
C-angle offset
Page 393
G996
Load monitoring
Page 389
G908
Feed rate override 100 %
Page 383
HEIDENHAIN MANUALplus 620, CNC PILOT 640
611
612
Overview of G codes
10.3 Overview of G commands in the MACHINING section
SYMBOLS
C
C
? – Simplified geometry
programming ... 194
"Configuration" pull-down menu ... 42
"Extras" pull-down menu ... 44
"Goto" pull-down menu ... 42
"Graphics" pull-down menu ... 45
"Head" pull-down menu (program
head) ... 41
"ICP" pull-down menu ... 41
"Miscellaneous" pull-down menu ... 43
"Program management" pull-down
menu ... 41
# variable output ... 406
C axis
C-angle offset G905 ... 393
Calibrate touch probe standard
G747 ... 473
Calibrate touch probe via two points
G748 ... 475
Cast part G21-Geo ... 200
C-axis commands ... 339
C-axis contours—Fundamentals ... 224
Centric polygon in XY plane G477Geo ... 512
Centric polygon in YZ plane G487Geo ... 520
Centric polygon milling—finishing
G844 ... 530
Centric polygon milling—roughing
G843 ... 529
Chamfer
DIN cycle G88 ... 438
Chamfer G88 ... 438
Character set ... 376
Chuck part
bar/tube G20-Geo ... 200
Chucking equipment in simulation
G65 ... 49, 381
Circular arc
DIN PLUS
Turning contour G2-, G3-, G12-,
G13-Geo ... 204, 205
Circular arc in face contour G102/G103Geo ... 232
Circular arc in lateral surface contour
G112/G113-Geo ... 241
Circular arc in XY plane G172-Geo/G173Geo ... 505
Circular arc in YZ plane G182-Geo/G183Geo ... 514
Circular arc of turning contour G12/G13Geo ... 205
Circular arc of turning contour G2/G3Geo ... 204
Circular arc on lateral surface G112/
G113 ... 347
Circular arc, face G102/G103 ... 343
Circular measurement ... 490
Circular measurement G785 ... 490
Circular movement G12, G13
(milling) ... 526
Circular movement G2, G3
(milling) ... 525
Circular path G12/G13 ... 252
Circular path G2/G3 ... 251
Circular pattern in XY plane G472Geo ... 511
Circular pattern in YZ plane G482Geo ... 519
Circular pattern on lateral surface G412Geo ... 247
Circular pattern with circular
slots ... 227
Circular pattern, face G745 ... 335
Circular pattern, lateral surface
G746 ... 337
Circular slot in XY plane G372-Geo/
G373-Geo ... 508
Circular slot in YZ plane G382-Geo/
G383-Geo ... 516
Circular slot on face G302/G303Geo ... 234
Circular slot on lateral surface G312/
G313-Geo ... 243
Codes, CONST ... 54
Codes, END ... 53
Codes, RETURN ... 53
Codes, VAR ... 54
Compensation of right/left-hand tool tip
G150/G151 ... 269
Compensation, additive G149 ... 268
Compensation, additive G149Geo ... 223
Compensations ... 266
Conditional block run ... 422
Configuration data, reading...—
PARA ... 418
Connection between geometry and
machining commands ... 444
Connection between geometry and
machining commands, C axis—front
face ... 445
Connection between geometry and
machining commands, C axis—lateral
surface ... 445
Connection between geometry and
machining commands, turning ... 444
CONST (section code) ... 54
Constant feed rate G94 ... 255
Constant surface speed Gx96 ... 256
Contour and figure milling cycle, face
G793 ... 351
A
Actual values in variable G901 ... 382
Additive compensation G149 ... 268
Additive compensation G149Geo ... 223
Address parameters ... 194
Angle offset
C-angle offset G905 ... 393
Angular ... 494
Angular measurement ... 494
Angular measurement G787 ... 494
ANUALplus ... 1
API thread G352 ... 312
Approach, departure in smart.Turn ... 65
Area milling, face G797 ... 355
Attributes for contour
description ... 220
Automatic working plan generation
(TURN PLUS) ... 553
AWG ... 553
B
B axis
Flexible use of tools ... 585
Fundamentals ... 584
Multipoint tools ... 586
Basic contour elements ... 201
Beginning of pocket/island G308Geo ... 224
BLANK (section code) ... 50
Bore hole (centric) G49-Geo ... 219
Bore hole on face G300-Geo ... 233
Bore hole on lateral surface G310Geo ... 242
Boring G72 ... 327
Boring, countersinking G72 ... 327
HEIDENHAIN MANUALplus 620, CNC PILOT 640
613
C
D
F
Contour and figure milling cycle, lateral
surface G794 ... 353
Contour follow-up ... 34, 380
Contour follow-up on/off G703 ... 380
Contour follow-up, saving/loading...
G702 ... 380
Contour form ... 62
Contour form elements ... 207
Contour milling G840 ... 358
Contour programming ... 191
Contour repeat cycle G83 ... 436
Contour thread ... 314
Contour, simple... G80 ... 294
Contour-based turning cycles ... 270
Contours in the XY plane ... 504
Contours in the YZ plane ... 513
Control graphics (TURN PLUS) ... 565
Controlled parting
Using lag error monitoring
G917 ... 396
Convert lengths G927 ... 385
Converting and mirroring G30 ... 389
Coolant
TURN PLUS machining
information ... 569
Countersinking G72 ... 327
Cut-off cycle G859 ... 315
Cutting data, determining (TURN
PLUS) ... 569
Cutting limit ... 503
Cutting speed, constant Gx96 ... 256
Cycle end / Simple contour G80 ... 294
Cycle, chamfer G88 ... 438
Cycle, radius G87 ... 438
Drilling cycle G71 ... 325
Drilling cycles
DIN programming ... 324
Drilling pattern, circular, face
G745 ... 335
Drilling pattern, circular, lateral surface
G746 ... 337
Drilling pattern, linear, face G743 ... 334
Drilling pattern, linear, lateral surface
G744 ... 336
Drilling, deep-hole drilling G74 ... 331
Feed per revolution Gx95 ... 255
Feed per tooth Gx93 ... 254
Feed rate ... 253
Feed rate override 100 % G908 ... 383
Feed rate reduction G38Geo ... 220, 221
Feed rate, interrupted G64 ... 254
Figure milling cycle, face G793 ... 351
Figure milling cycle, lateral surface
G794 ... 353
File organization, smart.Turn
editor ... 46
Find hole in C face G780 ... 482
Find hole in C lateral surface
G781 ... 484
Find stud in C face G782 ... 486
Find stud in C lateral surface
G783 ... 488
Finish contour G890 ... 290
Finishing
DIN PLUS
Cycle G890 ... 290
Fixed cycle programming (DIN
PLUS) ... 195
Fixed stop, traversing to G916 ... 394
Fluctuating spindle speed, reduce
resonant vibrations G924 ... 384
Force reduction G925 ... 397
Front face contours ... 230
Front face machining ... 341
Full circle in XY plane G374-Geo ... 508
Full circle in YZ plane G384-Geo ... 516
Full circle on face G304-Geo ... 235
Full circle on lateral surface G314Geo ... 244
Full-surface machining
In DIN PLUS ... 446
Full-surface machining with TURN
PLUS ... 578
D
Data input ... 405
Data output ... 405
Deburring G840 ... 365
Deep-hole drilling G74 ... 331
Detail, isolating
TURN PLUS ... 565
Determine pitch circle G786 ... 492
Dialog texts for subprograms ... 428
DIN PLUS workpiece blank
definition ... 200
DIN programs, converting ... 197
Direct program-run continuation ... 389
Drilling and boring cycles, overview and
contour reference... ... 324
614
E
Eccentric polygon in XY plane G377Geo ... 509
Eccentric polygon in YZ plane G387Geo ... 517
Eccentric polygon on front/rear face
G307-Geo ... 236
Eccentric polygon on lateral surface
G317-Geo ... 245
Eccentric turning G725 ... 399
Eccentric X G727 ... 403
Elements of a DIN program ... 37
END (section code) ... 53
End position of tool G922 ... 384
Engraving in the YZ plane G804 ... 540
Engraving in XY plane G803 ... 539
Engraving on front face G801 ... 378
Engraving on lateral surface
G802 ... 379
Engraving, character set ... 376
Example
Fixed cycle programming ... 195
Full-surface machining with
opposing spindle ... 448
Full-surface machining with single
spindle ... 450
Machining with the Y axis ... 544
Subprogram with contour
repetitions ... 441
TURN PLUS ... 574
Expert programs ... 196
F
Face roughing G820 ... 275
Face roughing, simple G82 ... 435
Feed per minute G94 ... 255
Feed per revolution G95 ... 255
Feed per revolution G95-Geo ... 223
G
G codes for contour description
G0 Starting point of turning
contour ... 201
G1 Line segment in a contour ... 202
G100 Starting point of front/rear
face contour ... 230
G101 Line segment in front/rear
face contour ... 231
G102 Circular arc in front/rear face
contour ... 232
G
G
G103 Circular arc in front/rear face
contour ... 232
G110 Starting point of lateral surface
contour ... 239
G111 Line segment in a lateral
surface contour ... 240
G112 Circular arc in lateral surface
contour ... 241
G113 Circular arc in lateral surface
contour ... 241
G12 Circular arc of turning
contour ... 205
G13 Circular arc of turning
contour ... 205
G149 Additive compensation ... 223
G170 Starting point of contour in XY
plane ... 504
G171 Line segment in XY
plane ... 504
G172 Circular arc in XY plane ... 505
G173 Circular arc in XY plane ... 505
G180 Starting point of contour in YZ
plane ... 513
G181 Line segment in YZ
plane ... 513
G182 Circular arc in YZ plane ... 514
G183 Circular arc in YZ plane ... 514
G2 Circular arc of turning
contour ... 204
G20 Chuck part bar/tube ... 200
G21 Cast part ... 200, 381
G22 recess (standard) ... 207
G23 recess (general) ... 209
G24 Thread with undercut ... 211
G25 Undercut contour ... 212, 432
G3 Circular arc of turning
contour ... 204
G300 Bore hole on front/rear
face ... 233
G301 Linear slot on front/rear
face ... 234
G302 Circular slot on front/rear
face ... 234
G303 Circular slot on front/rear
face ... 234
G304 Full circle on front/rear
face ... 235
G305 Rectangle on front/rear
face ... 235
G307 Eccentric polygon on front/
rear face ... 236
G
G308 Beginning of pocket/
island ... 224
G309 End of pocket/island ... 224
G310 Hole on lateral surface ... 242
G311 Linear slot on lateral
surface ... 243
G312 Circular slot on lateral
surface ... 243
G313 Circular slot on lateral
surface ... 243
G314 Full circle on lateral
surface ... 244
G315 Rectangle on lateral
surface ... 244
G317 Eccentric polygon on lateral
surface ... 245
G34 Thread (standard) ... 216
G37 Thread (general) ... 217
G370 Hole in XY plane ... 506
G371 Linear slot in XY plane ... 507
G372 Circular slot in XY plane ... 508
G373 Circular slot in XY plane ... 508
G374 Full circle in XY plane ... 508
G375 Rectangle in XY plane ... 509
G376 Single surface in XY
plane ... 512
G377 Eccentric polygon in XY
plane ... 509
G38 Feed rate reduction ... 220, 221
G380 Hole in YZ plane ... 515
G381 Linear slot in YZ plane ... 515
G382 Circular slot in YZ plane ... 516
G383 Circular slot in YZ plane ... 516
G384 Full circle in YZ plane ... 516
G385 Rectangle in YZ plane ... 517
G386 Single surface in YZ
plane ... 520
G387 Eccentric polygon in YZ
plane ... 517
G401 Linear pattern on front/rear
face ... 237
G402 Circular pattern on front/rear
face ... 238
G411 Linear pattern on lateral
surface ... 246
G412 Circular pattern on lateral
surface ... 247
G471 Linear pattern in XY
plane ... 510
G472 Circular pattern in XY
plane ... 511
HEIDENHAIN MANUALplus 620, CNC PILOT 640
G477 Centric polygon in XY
plane ... 512
G481 Linear pattern in YZ
plane ... 518
G482 Circular pattern in YZ
plane ... 519
G487 Centric polygon in YZ
plane ... 520
G49 Bore hole (centric) ... 219
G52 Blockwise oversize ... 222
G95 Feed per revolution ... 223
G codes for machining
G0 Rapid traverse ... 248
G0 Rapid traverse (Y axis) ... 523
G1 Linear movement ... 250
G1 Linear movement (Y axis) ... 524
G100 Rapid traverse on front/rear
face ... 341
G101 Line segment on front/rear
face ... 342
G102 Circular arc on front/rear
face ... 343
G103 Circular arc on front/rear
face ... 343
G110 Rapid traverse, lateral
surface ... 345
G111 Line segment on lateral
surface ... 346
G112 Circular arc on lateral
surface ... 347
G113 Circular arc on lateral
surface ... 347
G12 Circular movement (Y
axis) ... 526
G12 Circular path ... 252
G120 Reference diameter ... 339
G13 Circular movement (Y
axis) ... 526
G13 Circular path ... 252
G14 Approach tool change
point ... 249
G14 Approach tool change point (Y
axis) ... 523
G140 Definition of tool-change
point ... 249
G147 Safety clearance (milling
cycles) ... 265
G148 Switching the tool edge
compensation ... 267
G149 Additive compensation ... 268
615
G
G
G150 Compensation of right-hand
tool tip ... 269
G151 Compensation of left-hand
tool tip ... 269
G152 Zero point shift, C axis ... 339
G153 Standardize C axis ... 340
G16 Tilting the working plane ... 522
G17 XY plane ... 521
G18 XZ plane (turning) ... 521
G19 YZ plane ... 521
G2 Circular movement (Y
axis) ... 525
G2 Circular path ... 251
G26 Speed limitation ... 253
G3 Circular movement (Y
axis) ... 525
G3 Circular path ... 251
G30 Converting and mirroring ... 389
G301 Linear slot on face ... 295
G302 Circular slot on face ... 295
G303 Circular slot on face ... 295
G304 Full circle on face ... 296
G305 Rectangle on face ... 296
G307 Eccentric polygon on front/
rear face ... 297
G31 Thread cycle ... 303
G311 Linear slot on lateral
surface ... 297
G312 Circular slot on lateral
surface ... 298
G313 Circular slot on lateral
surface ... 298
G314 Full circle on lateral
surface ... 298
G315 Rectangle on lateral
surface ... 299
G317 Eccentric polygon on lateral
surface ... 299
G32 Single thread cycle ... 307
G33 Thread single path ... 309
G35 Metric ISO thread ... 311
G350 Simple longitudinal singlestart thread ... 439
G351 Simple longitudinal multi-start
thread ... 440
G352 Tapered API thread ... 312
G36 Tapping ... 330
G38 Metric ISO thread ... 314
G4 Period of dwell ... 381
G40 Switch off TRC/MCRC ... 257
G41 Switch on TRC/MCRC ... 258
616
G
G42 Switch on TRC/MCRC ... 258
G47 Safety clearance ... 265
G48 Reduce rapid traverse ... 253
G50 Switch off oversize ... 263
G51 Zero point shift ... 260
G53/G54/G55 Zero point
offsets ... 261
G56 Additive zero point shift ... 261
G57 Axis-parallel oversize ... 263
G58 Contour-parallel oversize ... 264
G59 Absolute zero point shift ... 262
G60 Switch off protection
zone ... 382
G64 Interrupted feed rate ... 254
G65 Chucking equipment ... 49, 381
G7 Precision stop on ... 381
G701 Rapid traverse to machine
coordinates ... 248
G701 Rapid traverse to machine
coordinates (Y axis) ... 523
G702 Saving/loading contour followup ... 380
G703 Contour follow-up ... 380
G71 Drilling cycle ... 325
G72 Boring, countersinking ... 327
G720 Spindle
synchronization ... 392
G725 Eccentric turning ... 399
G726 Transition to eccentric ... 401
G727 Eccentric X ... 403
G73 Tapping ... 328
G74 Deep-hole drilling ... 331
G740 Repeat recessing cycle ... 285
G741 Repeat recessing cycle ... 285
G743 Linear pattern, face ... 334
G744 Linear pattern, lateral
surface ... 336
G745 Circular pattern, face ... 335
G746 Circular pattern, lateral
surface ... 337
G791 Linear slot on face ... 349
G792 Linear slot on lateral
surface ... 350
G793 Contour and figure milling
cycle, face ... 351
G794 Contour and figure milling
cycle, lateral surface ... 353
G797 Area milling, face ... 355
G798 Helical-slot milling ... 357
G799 Thread milling, axial ... 338
G8 Precision stop off ... 382
G80 Cycle end / Simple
contour ... 294
G800 Thread milling in XY
plane ... 541
G801 Engraving on front face ... 378
G802 Engraving on lateral
surface ... 379
G803 Engraving in XY plane ... 539
G804 Engraving in YZ plane ... 540
G806 Thread milling in YZ
plane ... 542
G808 Hobbing ... 543
G809 Measuring cut ... 293
G81 Simple longitudinal
roughing ... 434
G810 Longitudinal roughing ... 272
G82 Simple face roughing ... 435
G820 Face roughing ... 275
G83 Contour repeat cycle ... 436
G830 Contour-parallel
roughing ... 278
G835 Contour-parallel with neutral
tool ... 281
G840 Contour milling ... 358
G841 Area milling—roughing (Y
axis) ... 527
G842 Area milling—finishing (Y
axis) ... 528
G843 Centric polygon milling—
roughing (Y axis) ... 529
G844 Centric polygon milling—
finishing (Y axis) ... 530
G845 Pocket milling,
roughing ... 368
G845 Pocket milling—roughing (Y
axis) ... 531
G846 Pocket milling,
finishing ... 374
G846 Pocket milling—finishing (Y
axis) ... 537
G85 Undercut cycle ... 316
G851 Undercut according to DIN
509 E with cylinder
machining ... 318
G852 Undercut according to DIN
509 F with cylinder
machining ... 319
G853 Undercut according to DIN 76
with cylinder machining ... 320
G856 Undercut type U ... 321
G857 Undercut type H ... 322
G
G858 Undercut type K ... 323
G859 Cut-off cycle ... 315
G86 Simple recessing cycle ... 437
G860 Contour-based
recessing ... 283
G869 Recess turning cycle ... 286
G87 Line with radius ... 438
G870 Recessing cycle ... 289
G88 Line with chamfer ... 438
G890 Finish contour ... 290
G9 Precision stop ... 382
G901 Actual values in
variables ... 382
G902 Zero-point shift in
variables ... 382
G903 Lag error in variables ... 382
G904 Read interpolation
information ... 383
G905 C-angle offset ... 393
G908 Feed rate override 100
% ... 383
G909 Interpreter stop ... 383
G916 Traversing to a fixed
stop ... 394
G917 Controlled parting ... 396
G919 Spindle override 100 % ... 383
G920 Deactivate zero-point
shifts ... 384
G921 Deactivate zero-point shifts,
tool lengths ... 384
G924 Fluctuating spindle
speed ... 384
G925 Force reduction ... 397
G93 Feed per tooth ... 254
G930 Sleeve monitoring ... 398
G94 Constant feed rate ... 255
G95 Feed per revolution ... 255
G96 Constant surface speed ... 256
G97 Speed ... 256
G976 Misalignment
compensation ... 387
G980 Activate zero-point
shifts ... 387
G981 Activate zero-point shifts, tool
lengths ... 387
G99 Workpiece group ... 391
G995 Monitoring zone
definition ... 388
G996 Type of load monitoring ... 389
G
L
G999 Direct program-run
continuation ... 389
G840—Calculating hole
positions ... 359
G840—Deburring ... 365
G840—Fundamentals ... 358
G840—Milling ... 361
G845—Calculating hole
positions ... 369
G845—Fundamentals ... 368
G845—Milling ... 370
Geometry commands ... 190
Global form ... 64
Global variables (DIN
programming) ... 408
Graphic, magnifying/reducing
TURN PLUS ... 565
L call ... 427
Lag error in variables G903 ... 382
Lateral surface
LATERAL_Y section ... 52
Lateral surface contours ... 239
LATERAL_Y—Section code ... 52
Lateral-surface machining ... 345
Line segment in a contour G1Geo ... 202
Line segment in a lateral surface
contour G111-Geo ... 240
Line segment in face contour G101Geo ... 231
Line segment in XY plane G171Geo ... 504
Line segment in YZ plane G181Geo ... 513
Linear and circular movements ... 250
Linear and circular movements in the Y
axis ... 524
Linear axes ... 36
Linear movement G1 ... 250
Linear movement G1 (milling) ... 524
Linear path, face G101 ... 342
Linear path, lateral surface G111 ... 346
Linear pattern in XY plane G471Geo ... 510
Linear pattern in YZ plane G481Geo ... 518
Linear pattern on lateral surface G411Geo ... 246
Linear pattern, face G743 ... 334
Linear pattern, lateral surface
G744 ... 336
Linear slot in XY plane G371-Geo ... 507
Linear slot in YZ plane G381-Geo ... 515
Linear slot on face G301-Geo ... 234
Linear slot on face G791 ... 349
Linear slot on lateral surface G311Geo ... 243
Linear slot on lateral surface
G792 ... 350
Local variables (DIN
programming) ... 408
Longitudinal roughing G810 ... 272
Longitudinal roughing, simple
G81 ... 434
H
Handwheel superposition
For G352 ... 313
Helical-slot milling G798 ... 357
Help commands for contour
definition ... 220
Help graphics for subprogram
calls ... 429
Hobbing G808 ... 543
Hole in XY plane G370-Geo ... 506
Hole in YZ plane G380-Geo ... 515
Hole positions, calculating, G840 ... 359
Hole positions, calculating... G845 (Y
axis) ... 532
I
IF.. Program branching ... 422
Inch conversion ... 385
Inch programming ... 36
Index of a parameter element,
determining...—PARA ... 419
In-process measurement ... 497
INPUT (input of # variable) ... 405
Input of variables—"INPUT" ... 405
Inside contours
TURN PLUS machining
information ... 569
Integer variables ... 407
Interpreter stop G909 ... 383
Interrupted feed G64 ... 254
Island (DIN PLUS) ... 224
HEIDENHAIN MANUALplus 620, CNC PILOT 640
617
M
M
P
M commands ... 430
M commands for program-run
control ... 430
M commands, machine
commands ... 431
Machine commands ... 431
Machining attributes for form
elements ... 201
Machining commands ... 190
Machining information (TURN
PLUS) ... 566
Machining sequence AWG
Editing ... 556
General ... 554
List of machining sequences ... 557
Managing ... 556
Magazine tool
Compensation in automatic
mode ... 587
Mathematical functions ... 407
MCRC, switch off...G40 ... 257
MCRC, switch on... G41/G42 ... 258
Measuring cut G809 ... 293
Menu structure, smart.Turn editor ... 38
Metric ISO thread G35 ... 311
Metric ISO thread G38 ... 314
Milling contour position ... 224
Milling cutter radius
compensation ... 257
Milling cycles for the Y axis ... 527
Milling cycles, overview... ... 348
Milling pattern, circular, face
G745 ... 335
Milling pattern, circular, lateral surface
G746 ... 337
Milling pattern, linear, face G743 ... 334
Milling pattern, linear, lateral surface
G744 ... 336
Milling, area milling, face G797 ... 355
Milling, contour and figure milling cycle,
face G793 ... 351
Milling, contour and figure milling cycle,
lateral surface G794 ... 353
Milling, contour milling G840 ... 358
Milling, G840—Fundamentals ... 358
Milling, helical-slot milling G798 ... 357
Milling, linear slot on face G791 ... 349
Milling, linear slot, lateral surface
G792 ... 350
Milling, pocket milling, finishing
G846 ... 374
Milling, pocket milling, roughing
G845 ... 368
Mirroring
DIN PLUS
Converting and mirroring
G30 ... 389
Misalignment compensation
G788 ... 496
Misalignment compensation, run
tapering operations G976 ... 387
Monitoring zone definition G995 ... 388
Multipoint tools ... 56
Multipoint tools for the B axis ... 586
Precision stop G9 ... 382
Precision stop off G8 ... 382
PRINT (output of # variable) ... 406
Probing ... 477
Probing in C axis G765 ... 478
Probing in two axes G766 ... 479
Probing in two axes G768 ... 480
Probing in two axes G769 ... 481
Program branching, IF ... 422
Program branching, SWITCH ... 425
Program branching, WHILE ... 424
Program conversion ... 196
Program example ... 441
Program section codes ... 47
Programming in DIN/ISO mode ... 190
Programming with variables ... 407
Protection zone, switch-off, G60 ... 382
Pull-down menus "Geometry" ... 199
Pull-down menus, "Units" ... 60
618
N
NC information, reading
general... ... 416
NC information, reading the
current... ... 414
NC program conversion ... 196
Nested contours ... 224
O
Operating modes
TURN PLUS ... 552
Output of # variables—"PRINT" ... 406
Output window for variables—
"WINDOW" ... 405
Oversize G52-Geo ... 222
Oversize, axis-parallel... G57 ... 263
Oversize, contour-parallel (equidistant)
G58 ... 264
Oversize, switch off... G50 ... 263
Oversizes ... 263
Overview form ... 61
P
Parallel editing ... 39
Parameter description—
subprograms ... 428
Paraxial probing G764 ... 477
Pattern, circular, on face G402Geo ... 238
Pattern, linear, on face G401Geo ... 237
Period of dwell G4 ... 381
Pocket milling, finishing G846 ... 374
Pocket milling, roughing G845 ... 368
Position of milling contours, Y
axis ... 502
Precision stop G7 ... 381
R
Radius G87 ... 438
Rapid traverse G0 ... 248
Rapid traverse G0, Y axis ... 523
Rapid traverse to machine coordinates
G701 ... 248
Rapid traverse, front face G100 ... 341
Rapid traverse, lateral surface
G110 ... 345
Rapid traverse, reducing... G48 ... 253
Reading diagnostic bits ... 413
Reading interpolation information
G904 ... 383
Reading tool data ... 410
Real variables ... 407
Rear-face machining
DIN PLUS
Example of full-surface
machining with opposing
spindle ... 448
Example of full-surface
machining with single
spindle ... 450
Recess (general) G23-Geo ... 209
Recess (standard) G22-Geo ... 207
Recess turning cycle G869 ... 286
Recessing cycle G870 ... 289
Recessing G86 ... 437
Recessing G860 ... 283
Recessing, recessing cycle G870 ... 289
R
S
S
Recessing, repeat recessing cycle
G740/G741 ... 285
Rectangle in XY plane G375-Geo ... 509
Rectangle in YZ plane G385-Geo ... 517
Rectangle on face G305-Geo ... 235
Rectangle on lateral surface G315Geo ... 244
Reference diameter G120 ... 339
Reference plane
LATERAL_Y section ... 52
Repeat recessing cycle G740/
G741 ... 285
Replacement tools ... 57
RETURN (section code) ... 53
Rotary axes ... 36
Roughing, contour-parallel G830 ... 278
Roughing, contour-parallel with neutral
tool G835 ... 281
Roughing, face G820 ... 275
Roughing, longitudinal G810 ... 272
Run-out length (thread) ... 300
Shaft machining (TURN PLUS)
Fundamentals ... 572
Simple turning cycles ... 434
Simplified geometry
programming ... 194
Simulation
TURN PLUS control graphics ... 565
Single surface in XY plane G376Geo ... 512
Single surface in YZ plane G386Geo ... 520
Single thread cycle G32 ... 307
Single-point measurement ... 457
Single-point measurement for zero
point G771 ... 459
Single-point tool compensation
G770 ... 457
Skip level ... 426
Sleeve monitoring G930 ... 398
Slot, circular, lateral surface G312/
G313-Geo ... 243
Slot, circular, on face G302/G303Geo ... 234
Slot, linear on lateral surface
G792 ... 350
Slot, linear, face G791 ... 349
Slot, linear, lateral surface G311Geo ... 243
Slot, linear, on face G301-Geo ... 234
smart.Turn editor ... 38
Speed ... 253
Speed Gx97 ... 256
Speed limitation G26 ... 253
Spindle
Spindle synchronization
G720 ... 392
Spindle override 100 % G919 ... 383
Standardize C axis G153 ... 340
Starting length (thread) ... 300
Starting point of contour in XY plane
G170-Geo ... 504
Starting point of contour in YZ plane
G180-Geo ... 513
Starting point of face contour G100Geo ... 230
Starting point of lateral surface contour
G110-Geo ... 239
Starting point of turning contour G0Geo ... 201
Structured NC program ... 35
Subprogram call
L"xx" V1 ... 427
Subprogram, dialogs texts in
subprogram call ... 428
Subprogram, help graphics for
subprogram calls ... 429
Subprograms—Fundamentals ... 196
SWITCH..CASE—program
branching ... 425
Synchronization
Synchronization, spindle
G720 ... 392
S
Safety clearance, milling cycles,
G147 ... 265
Safety clearance, turning cycles,
G47 ... 265
Screen layout, smart.Turn editor ... 39
Search cycles ... 482
Section codes, CONST ... 54
Section codes, END ... 53
Section codes, RETURN ... 53
Section codes, VAR ... 54
Sections, AUXIL_BLANK ... 50
Sections, AUXIL_CONTOUR ... 50
Sections, BLANK ... 50
Sections, FACE_C ... 51
Sections, FACE_Y ... 51
Sections, FINISHED ... 50
Sections, HEADER ... 48
Sections, LATERAL_C ... 51
Sections, MACHINING ... 53
Sections, REAR_C ... 51
Sections, REAR_Y ... 51
Sections, SUBPROGRAM ... 53
Sections, TURRET ... 50
Separation point
TURN PLUS machining
information ... 572
Separation point G44 ... 222
HEIDENHAIN MANUALplus 620, CNC PILOT 640
T
T command ... 266
T command, fundamentals ... 55
Tapered API thread G352 ... 312
Tapping G36—Single path ... 330
Tapping G73 ... 328
Thread (general) G37-Geo ... 217
Thread (standard) G34-Geo ... 216
Thread cycle G31 ... 303
Thread cycle, single G32 ... 307
Thread cycles ... 300
Thread milling in XY plane G800 ... 541
Thread milling in YZ plane G806 ... 542
Thread milling, axial G799 ... 338
Thread overrun ... 300
Thread single path G33 ... 309
Thread with undercut G24-Geo ... 211
Thread, metric ISO... G35 ... 311
Thread, tapered API... G352 ... 312
Tilted position of tool carrier ... 55
Tilted working plane—
fundamentals ... 584
Tilting the working plane G16 ... 522
Tool call T ... 266
Tool change point, moving
to...G14 ... 249
Tool commands ... 266
Tool edge compensation G148 ... 267
Tool edge compensation, switching
G148 ... 267
Tool entries, editing ... 56
Tool form ... 61, 66
Tool list, setting up ... 55
Tool positioning ... 248
Tool positioning in the Y axis ... 523
Tool programming ... 55
619
T
U
U
Tool selection
TURN PLUS ... 566, 578
Tool-change point,
definition...G140 ... 249
Tool-tip radius compensation ... 257
Touch probe calibration ... 473
Touch probe cycles ... 454
For automatic operation ... 456
Transition to eccentric G726 ... 401
TRC, switch off... G40 ... 257
TRC, switch on... G41/G42 ... 258
TURN PLUS
AWG
Editing and managing machining
sequences ... 556
List of machining
sequences ... 557
Machining sequence ... 554
Full-surface machining ... 578
General
Control graphics ... 565
Example ... 574
Machining information ... 566
Operating mode ... 552
Machining information
Cutting data ... 569
Inside contours ... 569
Shaft machining ... 572
Tool selection ... 566, 578
Turret assignment ... 566
Turning cycles, contour-based... ... 270
Turning cycles, simple... ... 434
Turret
TURN PLUS turret
assignment ... 566
Two-point measurement ... 465
Two-point measurement G17
G777 ... 469
Two-point measurement G18
longitudinal G776 ... 467
Two-point measurement G18
transverse G775 ... 465
Two-point measurement G19
G778 ... 471
Type of load monitoring G996 ... 389
Undercut according to DIN 76 with
cylinder machining G853 ... 320
Undercut contour G25 ... 432
Undercut contour G25-Geo ... 212
Undercut cycle G85 ... 316
Undercut cycles ... 316
Undercut DIN 509 E ... 213
Undercut DIN 509 F ... 213
Undercut DIN 76 ... 214
Undercut G85 ... 316
Undercut type H ... 214
Undercut type H G857 ... 322
Undercut type K ... 215
Undercut type K G858 ... 323
Undercut type U ... 212
Undercut type U G856 ... 321
Unit "API thread" ... 130
Unit "Bidirectional roughing in ICP" ... 70
Unit "C axis OFF" ... 161
Unit "C axis ON" ... 161
Unit "Centric boring" ... 83
Unit "Centric drilling" ... 80
Unit "Centric polygon milling, XY
plane" ... 178
Unit "Centric polygon milling, YZ
plane" ... 185
Unit "Centric tapping" ... 82
Unit "Circular pattern drilling, face" ... 88
Unit "Circular pattern drilling, lateral
surface" ... 97
Unit "Circular slot pattern, face" ... 135
Unit "Circular slot pattern, lateral
surface" ... 149
Unit "Circular tapping pattern,
face" ... 92
Unit "Circular tapping pattern, lateral
surface" ... 101
Unit "Contour milling, figures,
face" ... 139
Unit "Contour milling, figures, lateral
surface" ... 151
Unit "Contour recessing with direct
contour input" ... 75
Unit "Contour-parallel roughing in
ICP" ... 69
Unit "Deburring in XY plane" ... 180
Unit "Deburring in YZ plane" ... 187
Unit "Deburring, face" ... 146
Unit "Deburring, lateral surface" ... 158
Unit "Engraving in XY plane" ... 179
Unit "Engraving in YZ plane" ... 186
Unit "Engraving, face" ... 145
Unit "Engraving, lateral surface" ... 157
Unit "Face milling ICP" ... 137
Unit "Face milling" ... 136
Unit "Helical slot milling" ... 150
Unit "ICP boring/countersinking, C
axis" ... 105
Unit "ICP boring/countersinking, Y
axis" ... 170
Unit "ICP contour finishing" ... 118
Unit "ICP contour milling in XY
plane" ... 175
Unit "ICP contour milling in YZ
plane" ... 182
Unit "ICP contour milling, face" ... 141
Unit "ICP contour milling, lateral
surface" ... 153
Unit "ICP contour recessing" ... 73, 79
Unit "ICP drilling, C axis" ... 102
Unit "ICP drilling, Y axis" ... 168
Unit "ICP pocket milling in XY
plane" ... 176
Unit "ICP pocket milling in YZ
plane" ... 183
Unit "ICP pocket milling, face" ... 144
Unit "ICP pocket milling, lateral
surface" ... 156
Unit "ICP recess turning" ... 74
Unit "ICP tapping, C axis" ... 104
Unit "ICP tapping, Y axis" ... 169
Unit "ICP thread" ... 128
Unit "Linear pattern drilling, face" ... 86
Unit "Linear pattern drilling, lateral
surface" ... 95
Unit "Linear pattern tapping, front
face" ... 91
Unit "Linear slot pattern, face" ... 134
Unit "Linear slot pattern, lateral
surface" ... 148
Unit "Linear tapping pattern, lateral
surface" ... 100
Unit "Longitudinal finishing with direct
contour input" ... 120
Unit "Longitudinal roughing in ICP" ... 67
Unit "Longitudinal roughing with direct
contour input" ... 71
Unit "Measuring cut" ... 124
Unit "Parting" ... 77
Unit "Pocket milling, figures,
face" ... 142
U
Undercut ... 432
Undercut according to DIN 509 E with
cylinder machining G851 ... 318
Undercut according to DIN 509 F with
cylinder machining G852 ... 319
620
U
U
Z
Unit "Pocket milling, figures, lateral
surface" ... 154
Unit "Predrill, contour mill, figures on
face" ... 106
Unit "Predrill, contour mill, figures on
lateral surface" ... 112
Unit "Predrill, contour mill, ICP in XY
plane" ... 171
Unit "Predrill, contour mill, ICP in YZ
plane" ... 173
Unit "Predrill, contour mill, ICP on
face" ... 108
Unit "Predrill, contour mill, ICP on lateral
surface" ... 114
Unit "Predrill, pocket mill, figures on
face" ... 109
Unit "Predrill, pocket mill, figures on
lateral surface" ... 115
Unit "Predrill, pocket mill, ICP in XY
plane" ... 172
Unit "Predrill, pocket mill, ICP in YZ
plane" ... 174
Unit "Predrill, pocket mill, ICP on
face" ... 111
Unit "Predrill, pocket mill, ICP on lateral
surface" ... 117
Unit "Program beginning" ... 159
Unit "Program end" ... 164
Unit "Program section repeat" ... 163
Unit "Recess turning with direct contour
input" ... 76
Unit "Relief turns (undercut) type E, F,
DIN76" ... 122
Unit "Single hole, face" ... 84
Unit "Single hole, lateral surface" ... 93
Unit "Single-surface milling, XY
plane" ... 177
Unit "Single-surface milling, YZ
plane" ... 184
Unit "Slot, face" ... 133
Unit "Slot, lateral surface" ... 147
Unit "Subprogram call" ... 162
Unit "Tap hole, lateral surface" ... 99
Unit "Tapered thread" ... 131
Unit "Tapping, face" ... 90
Unit "Thread milling in XY plane" ... 181
Unit "Thread milling" ... 138
Unit "Thread, direct" ... 127
Unit "Tilt plane" ... 165
Unit "Transverse finishing with direct
contour input" ... 121
Unit "Transverse roughing in ICP" ... 68
Unit "Transverse roughing with direct
contour input" ... 72
Unit "Undercutting (H, K, U)" ... 78
Units of measure ... 36
UNITS—Fundamentals ... 60
using NC Start in single-block mode to
run NC blocks through to end of
program, G999 ... 389
Zero point offsets G53/G54/G55 ... 261
Zero point shift G51 ... 260
Zero point shift, absolute G59 ... 262
Zero point shift, additive G56 ... 261
Zero point shift, C axis G152 ... 339
Zero point shifts, overview... ... 259
Zero-point shift in variables G902 ... 382
Zero-point shifts, activating...
G980 ... 387
Zero-point shifts, deactivating,
G920 ... 384
Zero-point shifts, tool lengths,
activating... G981 ... 387
Zero-point shifts, tool lengths,
deactivating, G921 ... 384
V
VAR (section code) ... 54
Variable syntax, expanded... CONST –
VAR ... 420
Variable types ... 408
Variables
As address parameters ... 194
Variables, calculating automatically,
G940 ... 385
W
WHILE.. Program repeat ... 424
WINDOW (special output
window) ... 405
Working plan generation (TURN PLUS)
AWG ... 553
Working planes ... 521
Workpiece blank contour G67 (for
graphics) ... 381
Workpiece group G99 ... 391
Workpiece transfer
C-angle offset G905 ... 393
Controlled parting using lag error
monitoring G917 ... 396
Spindle synchronization
G720 ... 392
Traversing to a fixed stop
G916 ... 394
X
XY plane G17 (front or rear face) ... 521
XZ plane G18 (turning) ... 521
Y
Y-axis contours—Fundamentals ... 502
YZ plane G19 (plan view/lateral
surface) ... 521
HEIDENHAIN MANUALplus 620, CNC PILOT 640
621

 

  

 

  ­
­€ 
 
 
€

 
‚‚‚ƒ
ƒ
1118606-20 · Ver00 · SW03 · 11/2014 · H · Printed in Germany
*I_1118606-20*