6000M CNC Programming and Operations Manual - Acu-Rite

6000M CNC
Programming and Operations
Manual
www.anilam.com
CNC Programming and Operations Manual
P/N 70000487G - Warranty
Warranty
ANILAM warrants its products to be free from defects in material and workmanship for one (1)
year from date of installation. At our option, we will repair or replace any defective product
upon prepaid return to our factory.
This warranty applies to all products when used in a normal industrial environment. Any
unauthorized tampering, misuse or neglect will make this warranty null and void.
Under no circumstances will ANILAM, any affiliate, or related company assume any liability for
loss of use or for any direct or consequential damages.
The foregoing warranties are in lieu of all other warranties expressed or implied, including, but
not limited to, the implied warranties of merchantability and fitness for a particular purpose.
The information in this manual has been thoroughly reviewed and is believed to be accurate.
ANILAM reserves the right to make changes to improve reliability, function, or design without
notice. ANILAM assumes no liability arising out of the application or use of the product
described herein. All rights reserved. Subject to change without notice.
Copyright 2004 ACU-RITE Companies, Inc.
All rights reserved. Subject to change without notice.
17-April-04
iii
CNC Programming and Operations Manual
P/N 70000487G - Contents
Section 1 - Introduction
Effectivity Notation ............................................................................................................................. 1-1
Getting Started ................................................................................................................................... 1-2
Programming Concepts ..................................................................................................................... 1-3
Programs............................................................................................................................................ 1-3
Axis Descriptions................................................................................................................................ 1-3
X-Axis ............................................................................................................................................. 1-3
Y-Axis ............................................................................................................................................. 1-4
Z-Axis.............................................................................................................................................. 1-4
Defining Positions .............................................................................................................................. 1-4
Polar Coordinates........................................................................................................................... 1-5
Absolute Positioning....................................................................................................................... 1-5
Incremental Positioning.................................................................................................................. 1-6
Angle Measurement ........................................................................................................................... 1-6
Plane Selection .................................................................................................................................. 1-7
Arc Direction....................................................................................................................................... 1-8
Section 2 - CNC Console and Software Basics
The Console ....................................................................................................................................... 2-1
Keypad ............................................................................................................................................... 2-2
Alphanumeric Keys ........................................................................................................................ 2-2
Editing Keys.................................................................................................................................... 2-5
CNC Keyboard (Option) ..................................................................................................................... 2-5
Soft Keys (F1) to (F10)....................................................................................................................... 2-6
Manual Panel ..................................................................................................................................... 2-6
Software Basics ................................................................................................................................. 2-6
Pop-Up Menus................................................................................................................................ 2-6
Screen Saver.................................................................................................................................. 2-6
Clearing Entries .............................................................................................................................. 2-7
Operator Prompts ........................................................................................................................... 2-7
Cursor ............................................................................................................................................. 2-7
Typing Over and Inserting Text...................................................................................................... 2-7
Deleting Text .................................................................................................................................. 2-7
Messages/Error Messages ................................................................................................................ 2-8
Section 3 - Manual Operation and Machine Setup
Powering On the CNC........................................................................................................................ 3-1
Shutting Down the CNC..................................................................................................................... 3-1
Emergency Stop (E-STOP) .................................................................................................................. 3-1
Activating/Resetting the Servos ......................................................................................................... 3-2
Manual Panel ..................................................................................................................................... 3-2
Manual Panel Keys ........................................................................................................................ 3-3
Manual Panel LEDs........................................................................................................................ 3-4
Manual Mode Screen ......................................................................................................................... 3-5
Machine Status Display Area Labels ............................................................................................. 3-6
Program Area Labels ..................................................................................................................... 3-6
Manual Mode Settings ....................................................................................................................... 3-7
Activating Manual Mode Rapid or Feed......................................................................................... 3-8
Adjusting Rapid Move Speed......................................................................................................... 3-8
Absolute Mode.............................................................................................................................. 3-10
All rights reserved. Subject to change without notice.
17-April-04
v
CNC Programming and Operations Manual
P/N 70000487G - Contents
Jog Moves ........................................................................................................................................ 3-11
Changing the Jog Mode ............................................................................................................... 3-11
Selecting an Axis.......................................................................................................................... 3-11
Jogging the Machine (Incremental Moves).................................................................................. 3-12
Jogging the Machine (Continuous Moves) .................................................................................. 3-12
Manual Data Input Mode.................................................................................................................. 3-13
Using Manual Data Input Mode.................................................................................................... 3-13
Operating the Handwheel (Optional) ............................................................................................... 3-14
Section 4 - Preparatory Functions: G-Codes
Rapid Traverse (G0) .......................................................................................................................... 4-3
Linear Interpolation (G1) .................................................................................................................... 4-4
Angular Motion Programming Example............................................................................................. 4-5
Circular Interpolation (G2 and G3)..................................................................................................... 4-6
Examples of Circular Interpolation ................................................................................................. 4-7
Dwell (G4) ........................................................................................................................................ 4-10
Programming Non-modal Exact Stop Check (G9) .......................................................................... 4-11
Plane Selection (G17, G18, G19) .................................................................................................... 4-11
Setting Software Limits (G22) .......................................................................................................... 4-13
Returning to Reference Point (Machine Home) (G28) .................................................................... 4-15
Automatic Return from Reference Point (G29) ............................................................................... 4-16
Probe Move (G31)............................................................................................................................ 4-16
Fixture Offsets (Work Coordinate System Select), (G53) ............................................................... 4-17
Fixture Offset Table...................................................................................................................... 4-17
Activating the Fixture Offset Table............................................................................................... 4-17
Changing Fixture Offsets in the Table ......................................................................................... 4-18
Adjusting Fixture Offsets in the Table .......................................................................................... 4-18
Changing Fixture Offsets Using Calibrate Soft Keys................................................................... 4-18
G53 Programming Examples....................................................................................................... 4-18
Modal Corner Rounding/Chamfering (G59, G60)............................................................................ 4-19
In-Position Mode (Exact Stop Check) (G61) ................................................................................... 4-21
Automatic Feedrate Override for Arcs (G62, G63) .......................................................................... 4-21
Contouring Mode (Cutting Mode) (G64) .......................................................................................... 4-22
User Macros (G65, G66, G67)......................................................................................................... 4-22
Axis Rotation (G68).......................................................................................................................... 4-25
Activating Inch (G70) or MM (G71) Mode........................................................................................ 4-28
Axis Scaling (G72) ........................................................................................................................... 4-29
Activating Absolute (G90) or Incremental (G91) Mode ................................................................... 4-29
Absolute Zero Point Programming (G92) ........................................................................................ 4-30
Feed in IPM (G94)............................................................................................................................ 4-30
Feed Per Revolution (G95) .............................................................................................................. 4-31
Section 5 - Ellipses, Spirals, Canned Cycles, and Subprograms
Ellipses (G5)....................................................................................................................................... 5-1
Spiral (G6) .......................................................................................................................................... 5-3
Canned Cycles ................................................................................................................................... 5-4
Drilling, Tapping, and Boring Canned Cycles (G81 to G89) ............................................................. 5-5
Cancel Drill, Tap, or Bore Cycle (G80) .......................................................................................... 5-6
Spot Drilling (G81).......................................................................................................................... 5-6
Counterboring (G82) ...................................................................................................................... 5-6
Peck Drilling (G83) ......................................................................................................................... 5-7
Tapping (G84) ................................................................................................................................ 5-8
vi
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Contents
Boring, Bi-directional (G85)............................................................................................................ 5-9
Boring, Unidirectional (G86)........................................................................................................... 5-9
Chip Breaker Peck Cycle (G87)................................................................................................... 5-10
Flat Bottom Bi-Directional Boring (G89) ...................................................................................... 5-11
Drilling Example ........................................................................................................................... 5-11
Pattern Drill Cycles....................................................................................................................... 5-13
Bolt Hole Circle (G79) .................................................................................................................. 5-13
Hole Pattern (G179) ..................................................................................................................... 5-14
Pocket Cycles................................................................................................................................... 5-16
Draft Angle Pocket Cycle (G73) ................................................................................................... 5-17
Frame Pocket Milling (G75) ......................................................................................................... 5-19
Hole Milling (G76)......................................................................................................................... 5-21
Circular Pocket Milling (G77) ....................................................................................................... 5-23
Rectangular Pocket Milling (G78) ................................................................................................ 5-25
Area Clearance (Irregular) Pocket Milling (G169) ....................................................................... 5-27
Pockets with Islands (G162) ........................................................................................................ 5-29
Irregular Pocket Examples ........................................................................................................... 5-32
Facing Cycle (G170) .................................................................................................................... 5-34
Circular Profile Cycle (G171) ....................................................................................................... 5-36
Rectangular Profile Cycle (G172) ................................................................................................ 5-39
Thread Mill Cycle (G181) ............................................................................................................. 5-41
Plunge Circular Pocket Milling (G177)......................................................................................... 5-43
Plunge Rectangular Pocket Milling (G178).................................................................................. 5-45
Mold Rotation (G45) ..................................................................................................................... 5-46
Elbow Milling Cycle (G49) ............................................................................................................ 5-57
Subprograms.................................................................................................................................... 5-62
Subprogram Addresses ............................................................................................................... 5-62
Repetition of Subprogram (Loop)................................................................................................. 5-63
Calling a Subprogram from a Subprogram .................................................................................. 5-63
End of Subprogram (M99) with a P-Code.................................................................................... 5-67
Subprogram for Multiple Parts Programming .............................................................................. 5-67
Loop and Repeat Function........................................................................................................... 5-68
Section 6 - Program Editor
Activating the Program Editor ............................................................................................................ 6-1
Activating Edit Mode from the Manual Screen............................................................................... 6-1
Activating Edit Mode from the Program Directory ......................................................................... 6-1
Activating Edit Mode from Draw Graphics ..................................................................................... 6-1
Editing Soft Keys ................................................................................................................................ 6-2
Marking Programming Blocks............................................................................................................ 6-3
Unmarking Program Blocks ............................................................................................................... 6-3
Saving Edits ....................................................................................................................................... 6-4
Canceling Unsaved Edits................................................................................................................... 6-4
Deleting a Character .......................................................................................................................... 6-4
Deleting a Program Block .................................................................................................................. 6-4
Undeleting a Block ............................................................................................................................. 6-5
Canceling Edits to a Program Block .................................................................................................. 6-5
Inserting Text without Overwriting Previous Text .............................................................................. 6-5
Inserting Text and Overwriting Previous Text.................................................................................... 6-6
Advancing to the Beginning or End of a Block .................................................................................. 6-6
Advancing to the First or Last Block of a Program ............................................................................ 6-6
Searching the Program Listing for Selected Text.............................................................................. 6-6
All rights reserved. Subject to change without notice.
17-April-04
vii
CNC Programming and Operations Manual
P/N 70000487G - Contents
Going to a Block of the Program Listing ............................................................................................ 6-7
Replacing Typed Text with New Text ................................................................................................ 6-8
Scrolling Through the Program.......................................................................................................... 6-9
Paging through the Program.............................................................................................................. 6-9
Inserting a Blank Line ........................................................................................................................ 6-9
Abbreviating Statements.................................................................................................................. 6-10
Copying Program Blocks ................................................................................................................. 6-11
Pasting Blocks within a Program ..................................................................................................... 6-12
Recording Keystrokes ...................................................................................................................... 6-12
Retrieving Recorded Keystrokes ..................................................................................................... 6-12
Repeating a Command or Key ........................................................................................................ 6-13
(Re)numbering Program Blocks ...................................................................................................... 6-13
Printing the Entire Program.............................................................................................................. 6-14
Printing a Portion of a Program ....................................................................................................... 6-14
Accessing the Most Recently Used Programs ................................................................................ 6-15
Opening Another Program from the Program Listing...................................................................... 6-15
Copying Blocks to Another Program ............................................................................................... 6-16
Copying an Entire Program into Another Program.......................................................................... 6-16
Including Comments in a Program Listing....................................................................................... 6-17
Section 7 - Edit Help
Main Edit Help Menu.......................................................................................................................... 7-3
Help Template Menu.......................................................................................................................... 7-4
Help Graphic Screens .................................................................................................................... 7-6
Edit Help Soft Keys ............................................................................................................................ 7-7
Edit Help Menu................................................................................................................................... 7-8
Using Help Graphic Screens to Enter Program Blocks................................................................... 7-11
Line Moves ....................................................................................................................................... 7-13
Endpoint and Angle Calculation................................................................................................... 7-14
Arcs .................................................................................................................................................. 7-16
Multiple Move Commands ............................................................................................................... 7-22
Modal G-Code Box........................................................................................................................... 7-31
G-Code Listing ................................................................................................................................. 7-32
Entering a G-Code ........................................................................................................................... 7-32
Entry Fields ...................................................................................................................................... 7-33
M-Code Listing ................................................................................................................................. 7-34
Entering an M-Code ......................................................................................................................... 7-35
Typing in Address Words................................................................................................................. 7-35
Typing in M-Codes ........................................................................................................................... 7-36
Section 8 - Viewing Programs with Draw
Starting Draw...................................................................................................................................... 8-1
Draw Screen Description ................................................................................................................... 8-2
Putting Draw in Hold .......................................................................................................................... 8-3
Canceling Draw.................................................................................................................................. 8-3
Draw Parameters ............................................................................................................................... 8-4
Tool On or Off................................................................................................................................. 8-4
Drawing Compensated Moves ....................................................................................................... 8-5
Showing Rapid Moves.................................................................................................................... 8-5
Setting Grid Line Type.................................................................................................................... 8-6
Setting Grid Size............................................................................................................................. 8-6
Putting Draw in Motion, S.Step, or Auto Mode .............................................................................. 8-6
viii
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Contents
Automatic Draw Restart ................................................................................................................. 8-7
Erasing the Draw Display............................................................................................................... 8-7
Running Draw for Selected Blocks ................................................................................................ 8-8
Adjusting Draw Display ...................................................................................................................... 8-9
Fitting the Display to the Viewing Window..................................................................................... 8-9
Scaling the Display by a Factor...................................................................................................... 8-9
Using the Window Zoom .............................................................................................................. 8-10
Halving Display Size..................................................................................................................... 8-11
Doubling Display Size .................................................................................................................. 8-11
Changing the Viewing Area without Changing the Scale ............................................................ 8-11
Erasing Display............................................................................................................................. 8-12
Section 9 - Tool Page and Tool Management
Activating the Tool Page .................................................................................................................... 9-1
Using the Tool Page........................................................................................................................... 9-2
Finding Tools by Number................................................................................................................... 9-3
Changing Tool Page Values .............................................................................................................. 9-3
Clearing a Tool (Whole Row)......................................................................................................... 9-3
Clearing a Single Value.................................................................................................................. 9-3
Adjusting a Single Value ................................................................................................................ 9-3
Tool Page Soft Keys and Secondary Soft Keys ................................................................................ 9-5
T-Codes and Tool Activation.............................................................................................................. 9-5
Tool Definition Blocks..................................................................................................................... 9-6
Tool-Length Offsets............................................................................................................................ 9-6
Entering Offsets in the Tool Page .................................................................................................. 9-7
Setting Tool-Length Offsets ........................................................................................................... 9-8
Entering the Z Position Manually ................................................................................................... 9-9
Diameter Offset in Tool Page ............................................................................................................ 9-9
Tool Path Compensation (G41, G42) .......................................................................................... 9-11
Using Tool Diameter Compensation and Length Offsets with Ball-End Mills ............................. 9-14
Compensation (G40, G41, G42) ...................................................................................................... 9-15
Cancel Mode in Tool Compensation: G40.................................................................................. 9-15
Change of Tool Compensation Direction..................................................................................... 9-16
Startup and Movement in Z Axis .................................................................................................. 9-16
Temporary Change of Tool Diameter .......................................................................................... 9-17
Motion of Tool During Tool Compensation .................................................................................. 9-18
Compensation Around Acute Angles........................................................................................... 9-20
Change of Offset Direction........................................................................................................... 9-21
General Precautions..................................................................................................................... 9-22
G41 Programming Example......................................................................................................... 9-23
G42 Program Example................................................................................................................. 9-24
Activating Offsets via the Program .................................................................................................. 9-26
Section 10 - Program Management
Changing the Program Directory Display ........................................................................................ 10-2
Viewing All Programs of All Formats ............................................................................................... 10-2
Creating a New Part Program.......................................................................................................... 10-2
Choosing Program Names........................................................................................................... 10-3
Loading a Program for Running....................................................................................................... 10-3
Selecting a Program for Editing and Utilities ................................................................................... 10-3
Maximizing Program Storage Space ............................................................................................... 10-4
Displaying Program Blocks.............................................................................................................. 10-5
All rights reserved. Subject to change without notice.
17-April-04
ix
CNC Programming and Operations Manual
P/N 70000487G - Contents
Deleting a Program .......................................................................................................................... 10-5
Logging On to Other Drives ............................................................................................................. 10-6
Marking and Unmarking Programs.................................................................................................. 10-6
Marking Programs ........................................................................................................................ 10-6
Unmarking Marked Programs ...................................................................................................... 10-7
Marking All Programs................................................................................................................... 10-7
Unmarking All Marked Programs................................................................................................. 10-7
Deleting Groups of Programs .......................................................................................................... 10-7
Restoring Programs ......................................................................................................................... 10-8
Copying Programs to Floppy Disks ................................................................................................. 10-8
Renaming Programs ........................................................................................................................ 10-8
Printing Programs ............................................................................................................................ 10-9
Checking Disks for Lost Program Fragments.................................................................................. 10-9
Displaying System Information ...................................................................................................... 10-10
Using Wildcards to Find Programs ................................................................................................ 10-10
Copying Programs from/to Other Directories ................................................................................ 10-12
Renaming Programs from/to Another Directory ............................................................................ 10-12
Printing Programs from Another Drive/Directory ........................................................................... 10-13
Creating Subdirectories ................................................................................................................. 10-13
Deleting Programs on Another Drive ............................................................................................. 10-14
Listing a Program in Another Drive/Directory ................................................................................ 10-14
Editing a Program in Another Directory ......................................................................................... 10-15
Optimizing Your Hard Disk............................................................................................................. 10-15
Accessing the Disk Optimizer .................................................................................................... 10-15
Section 11 - Running Programs
Running a Program One Step at a Time ......................................................................................... 11-1
Switching Between Motion and Single-Step Mode...................................................................... 11-2
Holding or Canceling a Single-Step Run ..................................................................................... 11-2
Single-Step Execution of Selected Program Blocks.................................................................... 11-3
Position Display Modes.................................................................................................................... 11-4
Automatic Program Execution ......................................................................................................... 11-4
Holding or Canceling an Auto Run............................................................................................... 11-5
Starting at a Specific Block .......................................................................................................... 11-5
Clearing a Halted Program .............................................................................................................. 11-5
Using Draw while Running Programs.............................................................................................. 11-6
Setting the CNC to Display an Enlarged Position Display .............................................................. 11-7
Teach Mode ..................................................................................................................................... 11-7
Initiating Teach Mode ................................................................................................................... 11-8
Teach Mode Soft Keys ................................................................................................................. 11-8
Inputting Data with Teach Mode .................................................................................................. 11-9
Using Teach Mode ..................................................................................................................... 11-10
Exiting Teach Mode.................................................................................................................... 11-10
Parts Counter and Program Timer................................................................................................. 11-11
Jog/Return...................................................................................................................................... 11-13
Initiating Jog/Return ................................................................................................................... 11-13
Operations Allowed While “In” Jog/Return ................................................................................ 11-13
Jog/Return Soft Keys ................................................................................................................. 11-14
EXAMPLES: ............................................................................................................................... 11-16
Notes on Jog/Return .................................................................................................................. 11-18
x
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Contents
Section 12 - S and M Functions
Speed Spindle Control (S-Function)................................................................................................ 12-1
Miscellaneous Functions (M-Code) ................................................................................................. 12-2
Control M-Codes .............................................................................................................................. 12-2
Order of Execution ........................................................................................................................... 12-4
Section 13 - Communication and DNC
Communication ................................................................................................................................ 13-1
Installing the RS-232 Cable ............................................................................................................. 13-1
Accessing the Communication Software ......................................................................................... 13-2
Setting Communication Parameters................................................................................................ 13-3
Selecting the Communication Port............................................................................................... 13-3
Setting the Baud ........................................................................................................................... 13-3
Setting Parity ................................................................................................................................ 13-3
Setting Data Bits........................................................................................................................... 13-4
Setting Stop Bits ........................................................................................................................... 13-4
Software Setting ........................................................................................................................... 13-4
Setting Data Type......................................................................................................................... 13-5
Testing the Data Link ....................................................................................................................... 13-5
Activating the Test Link Screen ....................................................................................................... 13-6
Setting Test Link Display Modes.................................................................................................. 13-6
Testing the Link ............................................................................................................................ 13-7
Clearing the Receive Area ........................................................................................................... 13-7
Clearing the Transmit Area .......................................................................................................... 13-7
Sending a Program .......................................................................................................................... 13-7
Receiving a Program........................................................................................................................ 13-7
Setting the Transmission and Receiving Display ........................................................................ 13-8
Holding Transmission/Receiving Operations............................................................................... 13-8
Using Data Control (DC) Codes ...................................................................................................... 13-8
Using DC Codes In Receive Mode .............................................................................................. 13-9
Using DC Codes In Send Mode................................................................................................... 13-9
Accessing DNC .......................................................................................................................... 13-10
Section 14 - Machine Software and Peripherals Installation
Machine Software Installation .......................................................................................................... 14-1
Keyboard Installation (Option) ......................................................................................................... 14-1
Keypad Equivalent Keyboard Keys ................................................................................................. 14-2
Section 15 - Off-line Software
Passwords........................................................................................................................................ 15-1
Exiting the Software ......................................................................................................................... 15-1
Windows Off-line Software Installation............................................................................................ 15-2
Running Off-line Software from Windows.................................................................................... 15-2
System Settings ............................................................................................................................... 15-2
Maximum Memory Allocated........................................................................................................ 15-2
Disabled Features ........................................................................................................................ 15-3
Section 16 - Four-Axis Programming
Axis Types........................................................................................................................................ 16-1
Rotary Axis Programming Conventions........................................................................................... 16-2
Non-Synchronous or Synchronous Auxiliary Axis ........................................................................... 16-2
All rights reserved. Subject to change without notice.
17-April-04
xi
CNC Programming and Operations Manual
P/N 70000487G - Contents
Programming Examples................................................................................................................... 16-3
Example 1: Drill (Sync-Off).......................................................................................................... 16-4
Example 2: Mill (Sync-On) .......................................................................................................... 16-5
Example 3: Mill (Sync-On) .......................................................................................................... 16-6
Example 3: Mill (Sync-On) .......................................................................................................... 16-6
Section 17 - DXF Converter Feature
Requirements ................................................................................................................................... 17-1
Off-line Software........................................................................................................................... 17-1
Machine Software......................................................................................................................... 17-1
Entry to the DXF Converter.............................................................................................................. 17-2
Creating Shapes........................................................................................................................... 17-2
Contours ....................................................................................................................................... 17-3
Drilling........................................................................................................................................... 17-3
CNC Code ........................................................................................................................................ 17-3
Mouse Operations............................................................................................................................ 17-4
DXF Hot Keys................................................................................................................................... 17-5
Toggle Entity Endpoints (ALT + F)................................................................................................ 17-5
DXF Soft Keys.................................................................................................................................. 17-6
Miscellaneous DXF Soft Key, F6 ................................................................................................. 17-7
Output Menu Options ....................................................................................................................... 17-8
Shift X, Shift Y Descriptions ......................................................................................................... 17-8
Convert Polyline Description ........................................................................................................ 17-9
Display Menu Options ...................................................................................................................... 17-9
DXF Entities Supported ................................................................................................................. 17-10
Drawing Entities Not Supported ................................................................................................. 17-10
Files Created .................................................................................................................................. 17-11
DXF Example ................................................................................................................................. 17-11
Unedited Conversational Program Listing ................................................................................. 17-13
Unedited G-code Program Listing.............................................................................................. 17-14
Edited Conversational Program Listing ..................................................................................... 17-15
Edited G-code Tool Path ............................................................................................................ 17-16
Edited G-code Program Listing .................................................................................................. 17-17
Using DXF for Pockets with Islands (G162) .............................................................................. 17-18
Creating CAM Shapes ................................................................................................................... 17-21
Section 18 - CAM Programming
CAM Mode ....................................................................................................................................... 18-1
CAM Mode Soft Keys....................................................................................................................... 18-2
Shape (F2) Soft Keys ................................................................................................................... 18-3
Shape Edit Menu .......................................................................................................................... 18-4
Rev Arc............................................................................................................................................. 18-6
Delete ............................................................................................................................................... 18-6
Project .............................................................................................................................................. 18-6
Join ................................................................................................................................................... 18-7
Import ............................................................................................................................................... 18-7
View (F4) .......................................................................................................................................... 18-7
MOTION (F7) ................................................................................................................................... 18-8
Del Move (F8)................................................................................................................................... 18-8
Contour............................................................................................................................................. 18-8
xii
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Contents
Pocket............................................................................................................................................. 18-16
Pocket Menus Soft Keys ............................................................................................................ 18-22
Pockets with Islands (G162) ...................................................................................................... 18-23
Drill.............................................................................................................................................. 18-23
Edit.............................................................................................................................................. 18-26
Delete ......................................................................................................................................... 18-26
POST (F8) ...................................................................................................................................... 18-27
SETUP (F9).................................................................................................................................... 18-27
Shapes........................................................................................................................................ 18-28
Paths........................................................................................................................................... 18-29
Geometry .................................................................................................................................... 18-29
Post (F8) ..................................................................................................................................... 18-29
Posting Output Automatic Tool Changes................................................................................... 18-33
Exit (F10) ........................................................................................................................................ 18-34
Hot Keys ......................................................................................................................................... 18-34
Using the Shape Cursor................................................................................................................. 18-35
Selecting Editing Tools .................................................................................................................. 18-35
Line Tools....................................................................................................................................... 18-36
Arc Tools ........................................................................................................................................ 18-39
Corner Radius ................................................................................................................................ 18-41
Chamfering Corners....................................................................................................................... 18-41
Shape Edit Soft Keys ..................................................................................................................... 18-41
Reversing an Arc’s Direction...................................................................................................... 18-42
Deleting a Shape........................................................................................................................ 18-42
Projecting Line Segments (Restoring Sharp Corners) .............................................................. 18-42
Joining Line Segments............................................................................................................... 18-43
Importing Shapes from Other Programs.................................................................................... 18-43
Deleting a Segment.................................................................................................................... 18-43
Changing the CAM Mode View.................................................................................................. 18-44
Viewing a Listing of Shape Segment Details............................................................................. 18-44
Using Construction Geometry........................................................................................................ 18-46
Accessing Geometry Tools ............................................................................................................ 18-46
Point Tools.................................................................................................................................. 18-47
Line Tools ................................................................................................................................... 18-48
Circle Tools................................................................................................................................. 18-49
Notes on Geometry .................................................................................................................... 18-49
Chaining Geometry Elements to Create a Shape ......................................................................... 18-50
Viewing a Listing of Geometry Elements....................................................................................... 18-50
Deleting Geometry Elements ......................................................................................................... 18-51
Deleting All Geometry Elements.................................................................................................... 18-51
Managing Shape Files ................................................................................................................... 18-51
Using Shapes In G-code Programs ............................................................................................... 18-52
Sample Programs .......................................................................................................................... 18-52
Example #1 Machining an Outside Profile with Contour .......................................................... 18-52
Example #2 Machining a Slot using Contour............................................................................ 18-57
Example #3 Machining an Outside Profile using Contour........................................................ 18-60
Example #4 Machining a Contour with Many Unknown Intersections ..................................... 18-64
Example #5 Contour with Many Unknown Intersections - All Tangent Arcs ............................ 18-66
Example #6 Pocket Milled into Workpiece ............................................................................... 18-69
Example #7 Milled Pocket - X0 Y0 at Center of Radius ........................................................... 18-72
Example #8 Pocket Milled into Workpiece - X0 Y0 at Lower-Left Corner................................ 18-75
Example #9 Milled Pocket - X0 Y0 at the Center of the Large Radius .................................... 18-78
Example #10 Series of Holes using Drill .................................................................................. 18-80
All rights reserved. Subject to change without notice.
17-April-04
xiii
CNC Programming and Operations Manual
P/N 70000487G - Contents
Example #11 Pocket, Contour and Drill.................................................................................... 18-82
Example #12 Using CAM for Pockets with Islands (G162) ...................................................... 18-88
Additional Drawings for Practice ................................................................................................ 18-91
Section 19 - Advanced Programming Features
Modifiers........................................................................................................................................... 19-1
Block Separators.............................................................................................................................. 19-1
Tool Offset Modification ................................................................................................................... 19-2
Expressions and Functions.............................................................................................................. 19-4
Examples...................................................................................................................................... 19-5
System Variables ............................................................................................................................. 19-6
User Variables.................................................................................................................................. 19-8
Variable Programming (Parametric Programming) ..................................................................... 19-8
User Macros (G65, G66, G67)....................................................................................................... 19-14
Macro Body Structure................................................................................................................. 19-14
Setting and Passing Parameters ............................................................................................... 19-15
Probe Move (G31).......................................................................................................................... 19-23
Conditional Statements.................................................................................................................. 19-24
Unconditional LOOP Repeat ......................................................................................................... 19-25
Short Form Addressing .................................................................................................................. 19-26
Logical and Comparative Terms.................................................................................................... 19-27
Logical Terms ............................................................................................................................. 19-27
Comparative Terms.................................................................................................................... 19-27
File Inclusion .................................................................................................................................. 19-28
Index ...........................................................................................................................................Index-1
xiv
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Introduction
Section 1 - Introduction
This manual describes the concepts, programming commands, and CNC
programming formats used to program ANILAM CNC products. Use the
Contents and Index to locate topics of interest. In general, topics are
presented in order of complexity. For example, “Section 1” describes
basic CNC topics while later sections describe CAM programming and
special programming features that require a firm grasp of CNC
programming.
Effectivity Notation
Some sections of this manual apply only to specific ANILAM CNC
product(s). In these sections, icons in the left margin identify the
product(s) to which the information applies. Table 1-1 lists the icons for
each CNC product and the number of axes supported by each product.
Table 1-1, CNC Effectivity Icon Description
Icon
Product
6300M
6000M-3X
6000M-3X Systems
3
6000M-4X Systems
4
6000M-4X
6400M
Axes Supported
NOTE: All systems also support one spindle axis.
The main difference between the products is the number of axes
supported. Generally, this manual describes the 6000M-3X systems.
The 6000M-4X operates exactly as the 6000M-3X system except for
features that include the additional axes.
All rights reserved. Subject to change without notice.
17-April-04
1-1
CNC Programming and Operations Manual
P/N 70000487G - Introduction
Getting Started
Before you start to write a program, determine the work holding device
and the location of Part Zero (the point to which all movement is
referenced). Since absolute positions are defined from Part Zero, try to
select a location that directly corresponds to dimensions provided on the
part print, such as the lower left corner of the work. Then, you can
develop a program using a procedure similar to the one that follows:
1. To enter the Program Directory from the Manual screen, press
PROGRAM (F2). Create a program name for the part.
2. Enter the Program Editor (Edit F8) to open the new program and start
writing blocks.
3. The first block of any program is usually a safe start position and toolchange position (a position away from the work where the axes can
return for safe tool changing). The first block is normally also used to
specify the units of measurement (Inch/MM), mode of operation
(Absolute), move type (Rapid), and to cancel all auxiliary functions
(Tool Offsets, Spindle, and Coolant).
Typical first block:
G70 G90 G0 X0 Z0 T0 M5
4. Subsequent blocks in the program set Spindle information, call Tool
number, turn on Coolant, and make the initial move toward the work.
5. The remaining blocks in the program describe the required moves,
Canned Cycles, and Tool changes to complete the machining.
6. The next to the last block in the program returns the axes to the Tool
change position, turning off any auxiliary functions (Tool Offsets,
Spindle, and Coolant). The last block (M2) ends the program.
Typical final blocks:
M5
G0 T0 X0 Y0 Z0 M9
M2
7. After you write a program, verify it. Run it in Draw Graphics Mode to
troubleshoot for errors. Verify that all programmed moves are safe
and accurate to the part print dimensions.
8. Now, load the stock material into the selected work-holding device.
9. Set the Tool Offsets for each tool in the Tool Page.
10. Before running the part in the Auto Mode, run it in Single-Step Mode
to verify that both the program and the setting of Tool Offsets have
been correctly completed. Single-Step Mode allows you to execute
the program block-by-block.
11. After you test the program, make any necessary corrections.
12. When the finished program is ready for production, back it up on a
floppy disk.
1-2
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Introduction
Programming Concepts
This section contains programming concepts for the beginning
programmer. You must master these concepts and be familiar with the
terminology in order to write programs.
Programs
A program is the set of instructions that the CNC uses to direct the
machine movements. Each line of instructions is called a block. Each
block runs independently, thus allowing the program to be stepped along,
one block at a time.
Axis Descriptions
The machine moves along its axes of motion. All movements along an
axis are either in a positive or negative direction. Not all machines use
the same system to identify axes. The descriptions used in this manual
are commonly used to identify 3-axis mills.
NOTE: To visualize machine movements correctly, imagine tool motion
rather than table motion.
X-Axis
Table movement along the X-axis is to the left and right. Positive motion
is table movement to the left; negative motion is table movement to the
right. Refer to Figure 1-1.
Figure 1-1, Mill Axes of Motion
All rights reserved. Subject to change without notice.
17-April-04
1-3
CNC Programming and Operations Manual
P/N 70000487G - Introduction
Y-Axis
Table movement along the Y-axis is inward and outward. Positive motion
is table movement outward; negative motion is table movement inward.
Z-Axis
Spindle movement along the Z-axis is upward and downward. Positive
motion is tool movement upward (away from the workpiece); negative
motion is tool movement downward (into the workpiece).
Defining Positions
The intersection of the X-, Y-, and Z-axes is the reference point from
which to define most positions. Refer to Figure 1-2. This point is the X0,
Y0, Z0 position.
Most positions are identified by there X, Y, and Z coordinates. A position
two inches left, three inches back, and four inches up has an X
coordinate of X -2.0, a Y coordinate of Y3.0, and a Z coordinate of Z4.0.
Figure 1-2, Locating Positions
1-4
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Introduction
Polar Coordinates
Polar Coordinates define points that lie only on a single plane. Polar
coordinates use the distance from the origin and an angle to locate
points. Refer to Figure 1-3.
Figure 1-3, Polar Coordinate System
Absolute Positioning
In Absolute Mode, all positions are measured from Absolute Zero.
Absolute Zero is not a fixed position on the machine. It is a selected
point. Refer to Figure 1-4.
Figure 1-4, Absolute Positioning
You can set Absolute Zero (X0, Y0) anywhere. Usually, it is set at a
position that enables you to use the dimensions specified on the
blueprint. This is also called setting the Part Zero.
The Absolute Zero (Part Zero) can be moved as often as necessary,
either manually or in a program.
All rights reserved. Subject to change without notice.
17-April-04
1-5
CNC Programming and Operations Manual
P/N 70000487G - Introduction
Incremental Positioning
Incremental positions are measured from one point to another, or from
the machines present position. This is convenient for performing an
operation at regular intervals. Incremental positions are measured from
the tool’s present position. Refer to Figure 1-5.
NOTE: An incremental 0 inch (0 mm) move will not make a position
change because you are located at the 0 reference point
(current position).
Figure 1-5, Incremental Positioning
Angle Measurement
Angles are measured with the 3 o’clock position as the Zero Degree
Reference. Positive angles rotate counter-clockwise; negative angles
rotate clockwise. Refer to Figure 1-6.
Figure 1-6, Absolute Angle Measurement
1-6
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Introduction
Plane Selection
Circular moves and tool diameter compensation are confined to the plane
you select. Three planes are available: the XY plane (G17), the XZ plane
(G18), and the YZ plane (G19). It is important to view a plane correctly
when you plan a circular move. If a plane is viewed from the wrong side,
arc directions, angle references, and axis signs to appear reversed.
The standard rule is to view a plane looking in the negative direction
along the unused axis. Refer to Figure 1-7.
Figure 1-7, Plane Identification
All rights reserved. Subject to change without notice.
17-April-04
1-7
CNC Programming and Operations Manual
P/N 70000487G - Introduction
Arc Direction
The standard rule is to view arc direction for a plane from the positive
towards the negative direction along the unused axis. From this
viewpoint clockwise (Cw) and counterclockwise (Ccw) arc directions can
be determined. For example, in the XY plane, you view along the Z-axis,
from Z+ toward Z-, to determine Cw/Ccw directions. The Cw/Ccw arc
directions for each plane are shown in Figure 1-8.
Figure 1-8, Clockwise and Counterclockwise Arc Directions
1-8
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - CNC Console and Software Basics
Section 2 - CNC Console and Software Basics
The Console
The CNC console consists of a 12.1-inch color, flat-panel liquid crystal
display (LCD), keypad, soft keys, and manual panel. Refer to
Figure 2-1.
6000M
6300M
LCD
Keypad
Soft Keys
Manual
Panel
Figure 2-1, CNC Console
All rights reserved. Subject to change without notice.
17-April-04
2-1
CNC Programming and Operations Manual
P/N 70000487G - CNC Console and Software Basics
Keypad
Refer to Figure 2-2. The keypad to the right of the LCD has the following
areas:
Alphanumeric Keys: This area consists of the letters of the alphabet
listed sequentially from A to W, and also includes
the CLEAR key (lower right), the numerical keypad
(0 through 9) and the SPACE key (lower-left).
Edit Keys:
This area contains the SHIFT (left), ENTER (right)
and the cursor control keys (ARROWS).
Figure 2-2, Keypad
Alphanumeric Keys
Alphanumeric keys allow you to enter position coordinates (XYZ moves)
and program G, M, S, and T codes. Some keyfaces have two
characters, a large one in the middle of the key and a smaller one in the
upper-left corner. The large characters are Primary characters. The
smaller characters are SHIFT key characters.
2-2
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - CNC Console and Software Basics
To type a primary character, press the key that contains that character.
To type a SHIFT key character:
1. Press SHIFT. You do not need to hold down the key, it remains on
until you press the next key.
2. Press the key that displays the required character in the upper-left
corner. Refer to Table 2-1.
Table 2-1, Alphanumeric Keys
Key Face
Primary Function
SHIFT Function
Letter A
None
Letter B
Less Than Symbol
Letter C
Greater Than Symbol
Letter D
Caret
Letter E
None
Letter F/Feedrate
Left Bracket
Letter G/G Codes
Right Bracket
Letter H
Exclamation Point
Letter I
None
Letter J
Apostrophe
Letter K
Tilde Symbol
Letter L
“At” Symbol
Letter M
None
Miscellaneous
Functions
Letter N
Left Curly Bracket
Letter O
Right Curly Bracket
Program Number
Designator
Letter P
All rights reserved. Subject to change without notice.
17-April-04
Dollar Sign
2-3
CNC Programming and Operations Manual
P/N 70000487G - CNC Console and Software Basics
Key Face
2-4
Primary Function
SHIFT Function
Letter Q
None
Letter R
Underscore
Letter S/Spindle
Speed Designator
Backslash
Letter T/Tool words
Single Quote
Letter U
None
Letter V
Question Mark
Letter W
Colon
Letter X/X Axis
Coordinate
None
Letter Y/Y Axis
Coordinate
None
Letter Z/Z Axis
Coordinate
None
Number One
Left Parenthesis
Number Two
Right Parenthesis
Number Three
Pound or Number Sign
Number Four
Vertical Bar: used to separate
parts of a blueprint-programming
block for angles/chamfers/radii.
Number Five
Semi-Colon
Number Six
Slash
Number Seven
Ampersand
Number Eight
Percent Symbol
Number Nine
Inch Symbol
Number 0
Equal Sign
Minus Sign/Dash
Plus Sign
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - CNC Console and Software Basics
Key Face
Primary Function
SHIFT Function
Period/Decimal Sign
Asterisk: used to “comment out”
all or part of a block (characters to
the right of the asterisk are
ignored). The CNC ignores these
blocks.
Space Key
Blank Space
Editing Keys
Use the Editing Keys to edit programs and move around the screen.
Refer to Table 2-2.
Table 2-2, Editing Keys
Label or Name
Key Face
SHIFT
CLEAR
Purpose
Displays additional options on the soft
key menu. Allows access to additional
soft keys.
Clears selected messages, values,
commands and program blocks.
ARROW
Allows you to move highlight bars and
cursor around the screen.
ENTER
Activates menu selections, activates
alphanumeric entry, creates new line.
Use Editing Keys to control machine movements manually. Refer to
“Section 3 - Manual Operation and Machine Setup” for a detailed
description of the Manual Panel.
CNC Keyboard (Option)
The CNC supports most standard PC keyboards. Refer to “Section 14 Machine Software and Peripherals Installation.” All keypad inputs except
E-STOP and SERVO RESET have assigned keyboard equivalents.
All rights reserved. Subject to change without notice.
17-April-04
2-5
CNC Programming and Operations Manual
P/N 70000487G - CNC Console and Software Basics
Soft Keys (F1) to (F10)
Labeled soft keys F1 to F10, also called function keys, are located just
below the monitor. Soft key functions are not hardwired; their functions
change with changes in mode. Labels indicate the function of each soft
key. Unlabeled soft keys are inactive.
Manual Panel
Refer to “Section 3 - Manual Operation and Machine Setup” for
information on the manual panel and the optional handwheel.
Software Basics
The CNC’s screens change as different modes are activated. Basic
procedures and features of the software remain the same, regardless of
the CNC’s mode.
Pop-Up Menus
Pop-up menus are temporary menus that allow you to make additional
selections. Each pop-up menu contains a highlight bar. The ARROWS
move the highlight bar up and down the menu. Press ENTER to activate a
highlighted selection. Press the soft key again or press CLEAR to
deactivate the function. Refer to Figure 2-3.
Figure 2-3, Pop-Up Menu
Screen Saver
After a set period of inactivity, the CNC dims to preserve the LCD. The
CNC prompts you to press any key to restore its ready status.
2-6
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - CNC Console and Software Basics
Clearing Entries
Press CLEAR to clear an entry in an entry field, a line from a program, or a
message on the message line.
Operator Prompts
The CNC sometimes prompts for required information. Enter numbers
from the keypad.
Cursor
The CNC uses either a cursor or highlight to mark an item for selection or
editing. The highlight displays in the Edit Mode, Program Directory, and
Manual Mode. Use the ARROWS to move the highlight. The software
highlights a selected item in a menu or window. Selected items can be
activated or changed.
For instance, highlight a program block in Edit Mode to edit it. Highlight
an entry field label in a graphic menu to enter a value or toggle between
the available selections.
The cursor displays when the Tool Page activates. The cursor is a white
underline that indicates where letters and numbers will be inserted.
Typing Over and Inserting Text
The Editor has two text-entry modes, Typeover and Insert [Default:
Typeover]. In the Typeover mode, new characters replace characters
marked by the cursor.
In the Insert Mode, new characters appear at the cursor and existing
characters move to the right. When the Insert Mode is active, Ins (F3)
highlights. To put the CNC in the Insert mode:
1. When the CNC prompts for a name, press Ins (F3). The CNC
Highlights Ins (F3).
Deleting Text
To delete text:
1. Move the cursor to underline the text to be deleted.
2. Press Del (F4) to delete the selected text.
All rights reserved. Subject to change without notice.
17-April-04
2-7
CNC Programming and Operations Manual
P/N 70000487G - CNC Console and Software Basics
Messages/Error Messages
The CNC displays Messages it generates in the Message Area, present
in all program-running modes. When the CNC generates more than one
message, it displays the message with the highest priority in the Message
Area. Lower-priority messages remain in memory. Refer to Figure 2-4.
Figure 2-4, Messages Display
The on-screen MESSAGE label highlights when pending messages
remain in memory. You can review pending messages as follows:
q
Press CLEAR to clear the current message and display the next
message.
q
From the Manual screen, press MESSAGE (SHIFT + F1) to display
messages in the center of the screen.
Some messages are advisory, while others hold CNC
operation. For messages that halt operation, you must put the
CNC in the Manual Mode to correct the problem and clear the
message.
2-8
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Manual Operation and Machine Setup
Section 3 - Manual Operation and Machine Setup
Powering On the CNC
NOTE: When you power-on the CNC, ensure that the E-STOP switch is
in the in position.
1. Turn on the CNC according to the builder’s instructions. When the
power switch is turned on, the CNC completely resets.
2. Turn the power switch ON. The startup screen activates and prompts
you to Press F10 to continue.
3. Press (F10). The CNC displays the Software Options menu.
4. Highlight 1. CNC Control and press ENTER to activate Manual Mode.
Shutting Down the CNC
1. Press E-STOP to disengage the servos and revert to Manual Mode.
2. Press EXIT (SHIFT+F10) to display the Software Options menu.
3. Follow the builder’s instructions for turning off the CNC.
Emergency Stop (E-STOP)
Press E-STOP to take all axes and spindle servos offline. This ends all
machine movement.
To reset E-STOP, pull out and turn the rotary switch clockwise in the
direction of the arrows. The switch makes a clicking sound when it
resets.
Resetting E-STOP does not automatically reactivate the servos. The
servos must be reset to move the machine. Press SERVO RESET to reset
the servos.
All rights reserved. Subject to change without notice.
17-April-04
3-1
CNC Programming and Operations Manual
P/N 70000487G - Manual Operation and Machine Setup
Activating/Resetting the Servos
For safety reasons, the CNC powers up with the servomotors
disengaged. While the servos are off, the CNC cannot move the
machine. The CNC displays the message SERVO OFF! when the servos
are disengaged. The servos are also disengaged when you press
E-STOP, or if the machine attempts to travel beyond a limit switch.
Reset the servos as follows:
1. If a limit switch disengaged the servos, manually reposition the
machine inside its normal range of travel.
2. Press E-STOP to display MESSAGE: E-STOP IN-SERVO OFF!.
3. Rotate the E-STOP switch in the direction of the arrows to reset it. The
E-STOP switch makes a clicking sound when it resets.
4. Press SERVO RESET to display MESSAGE: SERVO DELAY, PLEASE
WAIT… while the CNC resets the servos. The message disappears
when the servos reset.
Manual Panel
Use the keys on the manual panel to move the machine manually. Refer
to Figure 3-1.
Figure 3-1, Manual Panel
3-2
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Manual Operation and Machine Setup
Manual Panel Keys
Manual panel keys allow you to control machine movements manually.
These keys are located on the Manual Panel. Refer to Table 3-1.
Table 3-1, Manual Operation Keys
Label/Name
Key Face
Handwheel
Axis Select
Purpose
Moves the selected controlled axis while in the Manual Mode.
Jog must be set to 1, 10, or 100. Optional.
Y
Z
U
X
In Manual Mode, selects the axis to be jogged.
AXIS
Cycles the CNC through manual movement modes (FEED,
RAPID, 100, 10, 1). The machine builder sets Default rapid
and feed rates at setup.
JOG
NOTE: The machine builder determines the actual speed of
the machine during a move.
SPINDLE
OVERRIDE
SPINDLE
FEEDRATE
OVERRIDE
Overrides the programmed spindle RPM rate. It is a
13-position rotary switch that ranges from 40 to 160 percent.
(Each increment adjusts the spindle override by 10%.) This
feature can be used only on machines with programmable
spindles.
Overrides the feed and/or rapid rate of the axes in Manual,
Auto, and Single Step modes. It is a 13-position rotary
switch, which ranges from 0 to 120 percent. (Each increment
adjusts the feedback override by 10%.)
NOTE: The override range for rapid rate is 100%. The CNC
will not exceed the maximum rapid rate.
SERVO RESET
Activates the servomotors.
SPINDLE
FORWARD
Starts the spindle in a forward direction.
SPINDLE
REVERSE
Starts the spindle in a reverse direction.
SPINDLE OFF
Stops the spindle.
START
Starts all machine moves except jog.
NOTE: On some machines, you must provide the gear range
and RPM before you activate this key.
NOTE: On some machines, you must provide gear range and
RPM before you activate this key.
(Continued…)
All rights reserved. Subject to change without notice.
17-April-04
3-3
CNC Programming and Operations Manual
P/N 70000487G - Manual Operation and Machine Setup
Table 3-1, Manual Operation Keys (Continued)
Label/Name
Key Face
Purpose
JOG -
Moves the selected axis in a negative direction. Available in
all modes. The machine builder specifies Feedrate.
HOLD
Halts any running program or programmed move. Press
START to continue.
E-STOP
Press E-STOP to halt all axes and machine-related functions.
When you activate E-STOP, the servomotors and any
programming operations shut down. The CNC defaults to
Manual Mode.
Use E-STOP for emergency shutdown or intentional servo
shutdown.
Manual Panel LEDs
The following keys have LEDs located directly above them on the Manual
Panel. When any of the keys is activated, the corresponding LED lights
up. Refer to Figure 3-1, Manual Panel.
q
q
q
q
Servo Reset
Spindle Off
Spindle Forward
Spindle Reverse
The Coolant Ready LED is also located on the Manual Panel. Some
CNCs have a coolant ready M-function. For these CNCs, the Coolant
Ready LED lights when the coolant is ready. The coolant is programmed
to come on when the machine receives a SPINDLE ON command.
3-4
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Manual Operation and Machine Setup
Manual Mode Screen
In Manual Mode, the CNC displays the Manual screen. The Manual
screen is the basic operating screen and is displayed when the CNC is
turned on. All other operating screens are similar in appearance and
selected from the Manual screen soft keys. When the Manual Mode is
active, the Manual (F4) soft key label highlights. Refer to Figure 3-2.
Program Area
Command Line
Message Line
Machine Position
Display
Motion Display
Area
Machine Status
Display Area
Active Soft Key
(Highlighted)
Figure 3-2, Manual Screen
The Manual screen is divided into the following areas.
Program Area
Displays the working program name, running
status, mode of operation, in-position check, and
command line.
Command Line
Allows you to enter commands manually.
Message Line
Displays messages, prompts, and reminders.
Machine Position Display
Displays machine’s X, Y, and Z position
coordinates in reference to Machine Home.
Motion Display Area
Displays machine’s X, Y, and Z position coordinates
in reference to:
q Part Zero
q Target
q Distance To Go
Machine Status Display Area
Displays operating information.
All rights reserved. Subject to change without notice.
17-April-04
3-5
CNC Programming and Operations Manual
P/N 70000487G - Manual Operation and Machine Setup
Active Soft Key
Identifies the function of the soft key. Soft key
functions change from screen to screen. A
highlighted label indicates an active mode.
Machine Status Display Area Labels
TOOL:
DIA:
LENG:
G:
M:
RPM:
FEED:
% RPM:
% Feed:
LOOP:
DWELL:
OVERRIDE:
PARTS:
TIMER:
FIXTURE:
Active tool.
Active tool diameter.
Z-Axis Tool-Length Offset for active tool.
Active G-Codes.
Active M-Codes.
Current spindle speed in revolutions per minute.
Current feed rate (in inch/mm per minute).
Spindle override setting (40% to 160%).
Feedrate override setting (0% to 120% for Feed moves
and 0% to 100% for Rapid moves).
Loop counter. Counts subprogram repetitions.
Seconds remaining in a dwell.
Indicates whether the feedrate override setting applies to
both feed and rapid moves or only to feed moves.
Number of parts. Resets to zero when you enter Auto or
Single Step mode.
Indicates the amount of time per part and accumulated
amount of time (in parentheses) for all parts. Resets to
zero when you enter Auto or Single Step mode.
Displays active fixture (G53).
Program Area Labels
Blk:
Block number (displays in S. Step or Auto Mode only).
PROGRAM:
Name of loaded program.
HALTED/*HALTED/RUNNING:
No asterisk:
Machine is in a programmed hold or has completed its
program.
With asterisk: External hold has been activated by an event or HOLD
was pressed.
RUNNING:
Program is running.
MANUAL/AUTO/S.STEP:
Current operating mode.
IN-POSN:
Displays if the machine has reached a programmed
endpoint.
COMMAND:
Enters commands in Manual Mode.
3-6
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Manual Operation and Machine Setup
Manual Mode Settings
Features (or settings) that remain active for more than one operation are
said to be modal. Modal features remain active until you change or
cancel them. Most CNC functions are modal.
For example, if the CNC is in Rapid Mode, it executes all moves at the
rapid rate until you initiate Feed Mode. The CNC can be in several
modes, as long as the modes do not conflict.
Before making a manual move, make any necessary mode settings.
Modes set from the Manual screen remain active if the CNC is put in a
program mode (Auto, S.Step) until the program or operator changes the
mode.
Set the following modes from the Manual screen:
q
q
q
q
Position Mode: Absolute or Incremental Mode
Move Mode: Rapid or Feed Mode
The Active tool: Active tool, tool-length offsets, and tool-nose radius
compensation
Measurement Mode: Inch or MM Mode
The Manual screen determines the following:
q
q
The location of Machine Home position
The location of Part Zero
Manual Mode provides the following types of moves:
q
q
q
q
Jog (Conventional)
Jog (Continuous)
Manual Data Input (MDI)
Handwheel (optional)
Table 3-2 describes the active soft keys in Manual Mode.
Table 3-2, Manual Mode Soft Keys
Label
Soft Key
Function
Help
F1
Activates the Help Mode.
Program
F2
Lists the user programs.
Edit
F3
Manual
F4
S.Step
F5
Activates the Edit Mode. A program
must first be selected.
Activates Manual Mode from Auto and
S.Step.
Changes to Single Step Mode.
Auto
F6
Delete
F7
All rights reserved. Subject to change without notice.
17-April-04
Changes to Auto Mode. Use to run part
programs for production.
Deletes a character from the command
line in Manual Mode.
3-7
CNC Programming and Operations Manual
P/N 70000487G - Manual Operation and Machine Setup
Table 3-2, Manual Mode Soft Keys (Continued)
Label
Soft Key
Insert
F8
Tool
F9
Handwheel
F10
Exit
SHIFT + F10
Message
F1
Teach
F5
Home
EXIT
F7
F10
Function
Puts the cursor in Insert Mode. Typed
text is inserted without overwriting the
existing text.
Displays the Tool Page. The Tool Page
stores tool diameter, length offsets, and
wear factors.
Activates or deactivates Handwheel
Mode. Use to jog any controlled axis in
Manual Mode.
Exits the Control Software and returns
to the Software options screen.
Displays the last 10 messages, both old
(already read) and new (not yet read).
Captures a display readout of axis
positions and saves it in a program.
Executes the machine homing function.
Quits the screen and returns to the
Software Startup menu.
Activating Manual Mode Rapid or Feed
Turn the JOG rotary switch to cycle through all available Jog Modes.
Choose Rapid or Feed mode. The CNC displays the active Feed or
Rapid Mode in the Machine Status Display Area.
NOTE: In Manual Mode, press R then press ENTER to toggle the
override setting between the following selections:
FEED and RAPID rate override (FEED, RAPID)
FEED rate override (FEED)
Toggle the setting to apply the current override selection to the
programmed rates.
Adjusting Rapid Move Speed
The FEEDRATE OVERRIDE rotary switch also adjusts the speed of Rapid
moves. If FEED, RAPID is set, every click of the FEEDRATE OVERRIDE
rotary switch adjusts the rapid rate by 10% of the default speed. The
switch provides a range of 0% to 100%. Set the switch to 100 to set the
rapid rate. The maximum override rate for rapid speeds is 100%.
NOTE: The machine builder determines the default rapid rate at setup.
3-8
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Manual Operation and Machine Setup
Absolute Mode
In Absolute Mode, all positions are measured from Absolute Zero.
Absolute Zero is X0, Y0, Z0 when the Absolute Mode is active. You can
move Absolute Zero to any convenient location. All absolute XYZ
positions are measured from this point. Refer to G53 and G92 in
“Section 4 - Preparatory Functions: G-Codes” for more information on
setting absolute zero. Setting Absolute Zero to a location on the part is
referred to as setting Part Zero. Refer to Figure 3-3.
Figure 3-3, Absolute Positioning
NOTE: To determine the Z-axis location of Part Zero, set tool length
offsets for each tool.
NOTE: The location of Absolute Zero can be restored after a shutdown
if the machine has the Home function installed.
CAUTION: If Part Zero is not correctly located, the CNC will not
position correctly in Absolute Mode.
All rights reserved. Subject to change without notice.
17-April-04
3-9
CNC Programming and Operations Manual
P/N 70000487G - Manual Operation and Machine Setup
Jog Moves
You can make or change jog moves when:
q
q
The CNC is in Manual Mode, the Teach Mode, or the Tool Page; and
The servos are on.
The actual rate for each mode is determined at machine setup. Use the
JOG rotary switch to cycle the CNC through the Jog Mode choices. Refer
to Table 3-3 for the available Jog Modes.
Table 3-3, Jog Modes
Mode
Rapid
Feed
Jog: 100
Jog: 10
Jog: 1
Description
Default rapid speed for continuous jogs. Actual speed
determined at machine setup.
Continuous jog at feedrate determined at machine setup.
Conventional Jog Mode, increment set to 100 times
machine resolution.
Conventional Jog Mode, increment set to 10 times machine
resolution.
Conventional Jog Mode, increment set to actual machine
resolution.
You can change the Jog Mode any time the CNC is in Manual Mode.
Changing the Jog Mode
NOTE: Jog move modes, with the exception of Jog Rapid Mode, are
performed in Feed Mode.
To change the Jog Mode:
1. In Manual Mode, turn the JOG switch to select a jog feed rate.
Selecting an Axis
To select an axis in the Manual Mode:
1. Use the AXIS SELECT rotary switch to cycle through the available axes.
Turn the switch until the indicator points to the required axis.
3-10
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Manual Operation and Machine Setup
Jogging the Machine (Incremental Moves)
In Manual Mode, position the machine with jog increments. To make a
jog increment move:
1. Use AXIS SELECT to select an axis.
2. Use JOG to cycle through the move mode choices and choose a Jog
Mode.
3. Press JOG+ or JOG- to choose a direction. Do not hold down the key.
Each time the key is pressed, the machine jogs along the selected
axis by the selected increment.
Jogging the Machine (Continuous Moves)
From the Manual screen, move the machine at feedrate or at the Jog
Rapid Rate. The machine builder determines the effective jog and feed
rates at setup.
1. In Manual Mode with the Manual screen active, use the AXIS SELECT
to select an axis.
2. Use JOG to select a Continuous Jog Mode (Feed or Rapid).
3. Press and hold down + or - to jog the machine in the desired
direction. The machine jogs along the selected axis. To stop the
machine, release the key.
All rights reserved. Subject to change without notice.
17-April-04
3-11
CNC Programming and Operations Manual
P/N 70000487G - Manual Operation and Machine Setup
Manual Data Input Mode
Manual Data Input (MDI) Mode allows you to command moves without
creating a part program. MDI also is a quick way to program one move,
or a series of moves that will be used only one time.
To execute a command, type an instruction on the COMMAND: line of
the Program Area, and press START. (In Manual Mode, the cursor rests
on the command line.)
More than one command can be programmed at a time. Use a
semicolon (;) to separate the commands.
Press HOLD to pause one-shot moves.
Press START to continue. Press Manual (F4) to cancel. MDI moves are
executed only once. To recall a previously commanded block, press UP
ARROW.
CAUTION: You must know the location of the Absolute Zero
before making Absolute Mode moves.
Using Manual Data Input Mode
To use Manual Data Input Mode:
1. In Manual Mode, type the command block(s) at the COMMAND: line.
2. Press START to execute the typed commands.
Most functions that can be commanded in a part program can also be
commanded in MDI Mode. These include:
q
q
q
q
G00, G01, G02, G03 moves
M-Codes, T-Codes (tool activation), S-Codes (spindle speed)
Modal commands (G90, G91, G70, G71, etc.)
G-Codes (G92, G28, G53, etc.)
The following example demonstrates how MDI Mode might be used to
activate the spindle.
COMMAND: M43; G97 S600; M3
M43
G97 S600
M3
3-12
Activates Gear Range defined by M43 in setup
Activates Specified Spindle Speed
Activates Spindle Forward
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Manual Operation and Machine Setup
Operating the Handwheel (Optional)
NOTE: The handwheel operation described here assumes that the
handwheel has been properly installed and configured in the
Setup Utility. The handwheel soft key will not display unless the
Setup Utility has been configured for handwheel use.
The CNC supports an option that allows you to move a selected axis via
a remote handwheel.
The resolution of the handwheel depends on the Jog Mode. Refer to
Figure 3-4.
Figure 3-4, Handwheel Operation
To select a Jog Mode:
1. Turn the rotary switch to select an axis.
2. Select a conventional Jog Mode (100, 10, or 1).
3. Press - or + to move in a negative or positive direction, respectively.
To operate the handwheel:
1. From the Manual screen, press HANDWHL (F10). The soft key
highlights and the other soft keys are blank.
2. On the Manual Panel, select the axis that will be moved using the
remote handwheel. Press ENTER. The selected axis can now be
moved using the remote handwheel.
3. On the Manual Panel, select a Jog Mode (100, 10, 1) at a speed
proportional to the 100, 10, and 1 setting.
All rights reserved. Subject to change without notice.
17-April-04
3-13
CNC Programming and Operations Manual
P/N 70000487G - Manual Operation and Machine Setup
4. Move the handwheel clockwise to move the selected axis in a positive
direction or counterclockwise to move the axis in a negative direction.
NOTE: If the axis does not move in the commanded direction, the
handwheel settings may need to be reconfigured in the Setup
Utility. Refer to the 6000M CNC Setup Utility Manual,
P/N 70000490, for details.
3-14
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Preparatory Functions: G-Codes
Section 4 - Preparatory Functions: G-Codes
G-codes initiate motion commands, canned cycles and various machine
and CNC functions. More than one G-code may be specified per block.
If a block contains conflicting G-codes, an Error message will appear.
Table 4-1 lists non-modal and modal G-codes. Modal G-codes remain in
effect until canceled by the appropriate code. Non-modal G-codes affect
only the block in which they are programmed.
Edit Help provides graphic menus and labeled entry fields to aid those
unfamiliar with G-code programming. Refer to “Section 7 - Edit Help” for
information.
Table 4-1, G-Codes
Modal
G-Code
Non-Modal
Function
Positioning-Rapid
Traverse
Linear Interpolation-Feed
Circular InterpolationCW
Circular InterpolationCCW
Stored Stroke Limit ON
G-Code
G4
G53
Tool Radius
Compensation, Cancel
Tool Radius
Compensation (Left)
Tool Radius
Compensation (Right)
Work Coordinate System
G59
Modal Corner Rounding
G63
G60
Modal Corner Rounding
Off
Exact Stop Check Mode
Cutting Mode
(Continuous Path ON)
User Macro Modal Call
G65
User Macro Modal Call
Cancel
G75
G0
G1
G2
G3
G22
G40
G41
G42
G61
G64
G66
G67
Function
Dwell
G5
G9
Ellipse
Exact Stop Check
G28
G31
Return to Machine
Home
Return from Machine
Home
Probe Move
G45
Mold Rotation
G49
Elbow Milling
G62
Automatic Feed
Override for Arcs
Automatic Feed
Override for Arcs
Cancel
User Macro Single Call
G29
G66
G67
G73
User Macro Modal Call
User Macro Modal Call
Cancel
Draft Pocket Milling
Cycle
Frame Milling
(Continued…)
All rights reserved. Subject to change without notice.
17-April-04
4-1
CNC Programming and Operations Manual
P/N 70000487G - Preparatory Functions: G-Codes
Table 4-1, G-Codes (Continued)
Modal
G-Code
G70
G71
Function
Coordinate System
Rotation (Axis Rotation)
Inch Programming
MM Programming
G72
Axis Scaling
G79
Circular Pocket Cycle
Rectangular Pocket
Cycle
Bolt Hole Circle Cycle
G81
G82
G80
G169
Cancel Modal Drilling
Area Clearance
G83
G84
Basic Drilling Cycle
Counterbore Drilling
Cycle
Basic Peck Cycle
Tapping Cycle
G170
G171
Facing Cycle
Circular Profile Cycle
G85
Basic Bore Cycle
G172
G86
Uni-directional Boring
Cycle
Chip Break Drilling Cycle
G177
Rectangular Profile
Cycle
Plunge Circular Pocket
Flat Bottom Bore Cycle
Absolute Programming
Incremental
Programming
Absolute Zero Preset
Per Minute Feed
Per Revolution Feed
G179
G181
G68
G87
G89
G90
G91
G92
G94
G95
4-2
Non-Modal
G-Code
G76
G77
G78
G178
Function
Hole Milling Cycle
Plunge Rectangular
Pocket
Hole Pattern Drilling
Thread Mill Cycle
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Preparatory Functions: G-Codes
Rapid Traverse (G0)
Format:
G0
G0 initiates rapid traverse. The machine builder sets the actual rapid rate
in the Setup Utility. Use rapid to position the tool prior to or after a cut.
Do not use rapid to cut a part. Refer to Figure 4-1.
One to four axes can be included on a block with G0. X, Y, and Z will
reach target simultaneously.
G0 is modal and remains in effect until canceled or changed.
Figure 4-1, Rapid Traverse
Table 4-2 lists the program blocks required to complete the moves
illustrated in Figure 4-1.
Table 4-2, Rapid Traverse
N1
G90 G0 X3 Y -1
N2
G1 X5.0
Rapid move to X3, Y-1 (P1) in
Absolute Mode.
X-axis feeds to X5 (P2).
N3
G0 X6 Y-2
XY rapid to X6, Y-2 (P3).
NOTE: To override rapid, use the FEEDRATE OVERRIDE. For more
information on using FEEDRATE OVERRIDE, refer to “Section 3 Manual Operation and Machine Setup.”
All rights reserved. Subject to change without notice.
17-April-04
4-3
CNC Programming and Operations Manual
P/N 70000487G - Preparatory Functions: G-Codes
Linear Interpolation (G1)
Format:
G1
Linear Interpolation (G1) initiates straight-line feed motion and is used to
cut a part. Straight-line motion occurs in one or more axes. The block
may contain any combination of available axes. G1 moves can be
straight-line or angular moves.
G1 is modal and remains in effect until changed. Specify the feedrate on
or prior to the G1 block.
In Figure 4-2 and Table 4-3, MM equivalents are in parentheses
following the Inch measurements.
Figure 4-2, Linear Motion
Table 4-3, Straight-Line Programming Example
4-4
N1
G90 G70 (G71) G1 X0 Y0 Z0
Feed to starting position.
N2
G1 F10 (254) X3.5 (88.9)
Feed to P2.
N3
Y-1.5 (-38.1)
Feed to P3.
N4
Z-1.5 (-38.1)
Move Z down.
N5
X0 (X0)
Feed to P4.
N6
Y0 (Y0)
Feed to P1.
N7
M2
End program, return to N1.
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Preparatory Functions: G-Codes
Angular Motion Programming Example
Angular moves involve motion in two or more axes. In Absolute Mode, all
dimensions are referenced to Part Zero (X0, Y0). In Incremental Mode,
all dimensions are referenced to the current tool position. Refer to
Table 4-4.
Table 4-4, Angular Programming Example, Absolute/Inch Mode
N1
G70 G90 G0 X0 Y0
Feed to starting position (X0, Y0).
N2
G1 F10 X3
Absolute, Inch Mode feed to P2.
N3
Y-2
Feed to P3.
N4
X0 Y-3
Feed to P4 (angular move).
N5
Y0
Feed to P1.
N6
M2
End program, return to N1.
In Figure 4-3, MM equivalents are in parentheses following the Inch
measurements.
Figure 4-3, Angular Motion
All rights reserved. Subject to change without notice.
17-April-04
4-5
CNC Programming and Operations Manual
P/N 70000487G - Preparatory Functions: G-Codes
Circular Interpolation (G2 and G3)
Circular interpolation initiates circular moves, including arcs. G2
commands a clockwise motion. G3 commands a counterclockwise
motion.
Arc input Format:
G2 Xx Yy Zz Ii Jj Kk
Arc input Format:
G3 Xx Yy Zz Ii Jj Kk
Radius Format:
G02 Xx Yy Rr
Radius Format:
G03 Xx Yy Rr
Refer to Table 4-5 for parameter descriptions.
NOTE: For circular interpolation in another plane, make the plane
changes prior to the G2 or G3 block. Refer to “Plane Selection
(G17, G18, G19)” for information on planes. Arc examples use
the most common plane, G17 (XY).
NOTE: If the value of X, Y, Z, I, J, or K is zero, omit it.
Table 4-5, Parameters for Circular Interpolation
Parameter
G2
G3
XYZ
I (X)
J (Y)
K (Z)
R
4-6
Description
CW (clockwise) motion.
CCW (counterclockwise) motion.
Endpoint of arc motion in Absolute or Incremental Mode.
Distance from the tool location to the arc center. I = X
center, J = Y center, and K = Z center.
NOTE: Arc centers are incremental by default. This is set
up in the Setup Utility.
Arc Radius.
NOTE: If Arc is greater than 180°, enter the R-value as a
negative value (For example, R-.5).
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Preparatory Functions: G-Codes
Examples of Circular Interpolation
Partial Arcs (XYIJ)
Figure 4-4 illustrates an arc move between P2 and P3.
4.5” (114.3 mm)
.5”
(12.7 mm)
2.5”
(63.5 mm)
Figure 4-4, Circular Interpolation
Absolute Mode: Refer to Table 4-6.
Table 4-6, Circular Interpolation in Absolute Mode, Inches
Address Word
Format
Description
N1
G70 G90 G17 G1 Y2.5 F3
N2
G2 X.5 Y3.0 I.5 J0
Activate Inch and Absolute
Mode and set feedrate to IPR.
Activate plane. Feed to P2.
Arc move to P3.
N3
G1 X5
Feed to P4.
N4
Y0
Feed to P5.
N5
X0
Feed to P1.
N6
M2
End Program.
Incremental Mode: Refer to Table 4-7.
Table 4-7, Circular Interpolation in Incremental Mode, Inches
Address Word
Format
N1
G70 G91 G17 G1 Y2.5 F3
N2
G2 X.5 Y.5 I.5 J0
Activate Inch and Absolute
Mode and set feedrate to IPR.
Activate plane. Feed to P2.
Arc move to P3.
N3
G1 X4.5
Feed to P4.
N4
Y-3
Feed to P5.
N5
X-5
Feed to P1.
N6
M2
End Program.
All rights reserved. Subject to change without notice.
17-April-04
Description
4-7
CNC Programming and Operations Manual
P/N 70000487G - Preparatory Functions: G-Codes
Any arc of less than 360 degrees is a partial arc. Use Address Words X,
Y, I, J together.
To program a move from P1 to P2, calculate arc centers (I and J) and
endpoints (X and Y). Refer to Figure 4-5.
Figure 4-5, Partial Arc Sample
From P1 to P2, the block format is: G91 G3 X.5559 Y.7244 I-.1941
J.7244.
Construct a triangle at a right angle to the given angle (15 deg.). Using
the given angle (15) and the hypotenuse (.75, radius), calculate the
lengths of the unknown sides I (opposite side) and J (adjacent side).
A. Sine (15 deg.) times hypotenuse = I
.2588 x .75 = .1941
Since I is in an X minus direction, I (X arc center) = -.1941
B. Cosine (15 deg.) times hypotenuse = J
.9659 x .75 = .7244
Since J is in a Y positive direction, J (Y arc center) = .7244
C. Radius - I = X
.750 - .1941 = .5559
X moves in a positive direction. X (endpoint) = .5559
D. Y (endpoint) = J (Y arc center)
Y = J = .7244
NOTE: If the endpoint (P2) does not lie along the arc path, the CNC
displays an error message.
4-8
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Preparatory Functions: G-Codes
Circles
Since the endpoint and starting point of a circle are the same, you do not
need to program an endpoint for a circle. Position the tool at the required
starting point before you execute the arc move. Refer to
Figure 4-6.
Format:
G91 G3 J.5
Since X, Y, and I equal 0, omit these parameters.
Figure 4-6, Circle Sample
Helical Interpolation (XYZIJK)
Format:
G17 G2 Xn Yn Zn In Jn Ln
Helical interpolation adds a third dimension to G2 or G3 moves.
For the XY plane (G17), the tool will move in a circular motion in the XY
axes and linearly in Z, simultaneously.
The added Z parameter provides the Z endpoint. L is the number of
complete plus partial revolutions, referenced from the start point.
You can use helical interpolation for threading and rough boring
applications. Additional linear or rotary axes (U, W) can also be
specified. Refer to Table 4-8.
Table 4-8, Helical Interpolation Program
Block
N5 G17 G90 G70 G0 X0 Y0 Z0
N6 G02 X2.0 Y0 Z-.5 I1.0 J0 L1 F20
N7 G01
All rights reserved. Subject to change without notice.
17-April-04
Description
Sets XY plane, Absolute, Inch, Rapid
Modes. Moves axes to zero.
Programs CW helical move to X2 Y0 Z-.5,
with center point at I1J0 and 0 complete
turns. The tool will execute a half turn at
feedrate F20. If L2 were programmed, the
tool would make 1-1/2 turns.
Next block.
4-9
CNC Programming and Operations Manual
P/N 70000487G - Preparatory Functions: G-Codes
Dwell (G4)
Dwell (G4) can be used to program a delay between blocks. A Timed
Dwell is a timed stop. An Infinite Dwell is a stop that can be canceled
only by pressing START. With a dwell activated, the CNC halts motions
on all axes, but other functions (coolant on/off, spindle control) remain
active. Do not program any other commands on a G4 block. T is the
time in seconds that the machine will remain at the current location. The
range of T is .1 to 9999.9 seconds.
Timed Dwell Format: G4 Tx.x (timed)
Infinite Dwell Format: G4 T0 (infinite)
Example:
N20 G4 T2.1
Block 20 commands a timed dwell with duration of 2.1 seconds.
Example:
N21 G4 T0
Block 21 commands an infinite dwell.
The time countdown is displayed in the Machine Status Area of the
Manual screen.
NOTE: ANILAM recommends that you use the Programmed Stop
M-function (M00) instead of an infinite dwell.
4-10
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Preparatory Functions: G-Codes
Programming Non-modal Exact Stop Check (G9)
With the In-Position Mode activated, the CNC approaches target and
performs an in-position check before it executes the next move. The
CNC comes to a complete stop at the end of every block. This could
cause witness marks to appear on the work, but prevents the CNC from
rounding off sharp corners. Refer to Table 4-9.
Format:
G9
NOTE: Rapid moves are always performed in In-Position Mode.
Table 4-9, Exact Stop Check G-Codes
Code
Format
G9
G9 Xx.x Yx.x
G61
G61 Xx.x Yx.x
G64
G64
Action
Activates non-modal In-Position Mode.
Complete stop only in this block.
Activates Modal In-Position Mode. The
CNC stops to verify location for each
targeted position. In-Position Mode
remains active until changed.
Cancels G61 and activates the Contouring
Mode (also called Continuous Path Mode).
NOTE: In-Position and Continuous Path Tolerances are defined in the
Setup Utility. The In-Position Tolerance should be closer to
target than the Continuous Path Tolerance.
The In-Position Mode will be active only for the block containing the G9
command. Use G61 to initiate modal Exact Stop Check (In-Position
Mode).
Plane Selection (G17, G18, G19)
Make plane changes prior to circular interpolation (G02, G03) blocks.
Refer to Table 4-10 for the G-codes that activate different planes. XY
(G17) is the default plane at power-on. Refer to Figure 4-7, Plane
Selection.
Table 4-10, Plane Selection G-codes
G-Code
G17
G18
G19
Cutting Plane
XY plane
XZ plane
YZ plane
All rights reserved. Subject to change without notice.
17-April-04
4-11
CNC Programming and Operations Manual
P/N 70000487G - Preparatory Functions: G-Codes
Figure 4-7, Plane Selection
To determine arc direction, look toward the negative direction of the nonused axis. Refer to Figure 4-8. (Example: for XY plane, look along Z-.)
Figure 4-8, Arc Direction
4-12
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Preparatory Functions: G-Codes
Setting Software Limits (G22)
The G22 Xn Yn Zn In Jn Kn format (activate software limits) is modal.
Use G22 (alone) to cancel software limits. Refer to Table 4-11.
Format:
G22 Xn Yn Zn In Jn Kn
Activates software limits.
Format:
G22
Cancels software limits and enables free movement within
the machine limits.
Table 4-11, G22 Address Words
Address Word
G22
X
Y
Z
I
J
K
Format
--xxx.xxxx
xxx.xxxx
xxx.xxxx
xxx.xxxx
xxx.xxxx
xxx.xxxx
Description
Stored Stroke Limit
(Programmable Travel Limits)
X positive software limit.
Y positive software limit.
Z positive software limit.
X negative software limit.
Y negative software limit.
Z negative software limit.
The software limits feature creates an envelope that limits the tool’s
range of travel. It is also called the Stored Stroke Limit feature. The X,
Y, and Z limits represent the extreme distance the tool can travel in the
positive X, Y, and Z directions. The I, J, and K limits represent the
extreme distance the tool can travel in the negative X, Y, and Z
directions. Refer to
Figure 4-9.
Software limits are referenced to Absolute Zero (Machine Home). The
values of the positive and negative limits depend on where you locate
Machine Home.
Figure 4-9, Software Limits Envelope Parameters
All rights reserved. Subject to change without notice.
17-April-04
4-13
CNC Programming and Operations Manual
P/N 70000487G - Preparatory Functions: G-Codes
To set software limits:
1. Make sure the tool is within the envelope defined by the software
limits (XYZIJK).
2. In Edit Mode or Manual Mode, type the G22 command in the proper
format (G22 Xn Yn Zn In Jn Kn). All the Address Words must be
accompanied by the appropriate values or the CNC will not activate
software limits.
In Edit Mode, make sure the appropriate Program Listing is displayed.
Type the G22 command into any program block.
In the Manual Mode, type the G22 command next to the command
line. Press START.
4-14
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Preparatory Functions: G-Codes
Returning to Reference Point (Machine Home) (G28)
With the G28 XYZ format, the Machine Home command (G28) returns
the CNC to a permanent reference position and sets the Absolute Zero
Reference at that point. The G28 command is used to zero the machine
after a shutdown. Refer to Table 4-12.
Format:
G28 XYZ
Returns the machine directly to its X, Y, and Z reference
point (Machine Home). The axes display will zero when
the reference point is reached.
Format:
G28 Xn Yn Zn
n = coordinates X, Y, and Z of intermediate point. Return
to reference point (Machine Home) through an
intermediate point.
Table 4-12, Return to Reference Point, Address Words
Address Word
G28
Xn
Yn
Zn
NOTE:
Format
--xxx.xxxx
xxx.xxxx
xxx.xxxx
Description
Return to Reference point, directly or
through an intermediate point
Intermediate point in X, if used
Intermediate point in Y, if used
Intermediate point in Z, if used
At least one axis must be specified, or no motion will occur.
The order in which the axes return to the reference point is determined at
setup by the machine builder. With the G28 Xx Yy Zz format, the
machine rapids to the intermediate point and then feeds to Machine
Home. The intermediate point is always in reference to Machine Home.
NOTE: All homing motion will be at a rate set by parameter.
Be sure to cancel Tool Diameter Compensation (G41 and G42) before
commanding G28. Tool Length Offsets are automatically canceled by
G28 XYZ.
All rights reserved. Subject to change without notice.
17-April-04
4-15
CNC Programming and Operations Manual
P/N 70000487G - Preparatory Functions: G-Codes
Automatic Return from Reference Point (G29)
Automatic Return from Reference Point (Machine Home) (G29) is used in
conjunction with Machine Home (G28). G29 returns the CNC to the
intermediary point programmed in G28, then to the coordinates
programmed in the G29 block. It can be used to return from the
reference point to a program start position. Refer to Table 4-13.
Format:
G29 Xx Yy Zz
xyz = coordinates X, Y, and Z of G29 move. The CNC
commands a move from Machine Home to an intermediate
point (specified in G28 command), then to the G29
coordinates.
Table 4-13, G 29 Address Words
Address Word
Description
G29
Return from Machine Home, through an
intermediate point specified in the G28 command, to
the G29 programmed coordinates.
G29 move in X
G29 move in Y
G29 move in Z
X
Y
Z
NOTE: If the G28 move is to Machine Home, enter the command as
follows: G28 X0 Y0 Z0 or G28 XYZ. The axes address words
must be specified or the CNC will not home the omitted axis.
Refer to Table 4-14.
Table 4-14, G29 Program List
Block
Format
N1
G28 Xx1 Yy1 Zz1
N2
G29 Xx2 Yy2 Zz2
Description of Variables
N1 = coordinates of intermediary point.
The CNC rapid to the programmed
coordinate (N1), then feeds to Machine
Home.
N2 = coordinates of point to which CNC
will return after reaching the intermediary
point. The machine feeds to the G28
intermediate point (N1), then to the
programmed coordinate (N2).
Probe Move (G31)
Refer to “Section 19 - Advanced Programming Features,” “Probe Move
(G31).”
4-16
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Preparatory Functions: G-Codes
Fixture Offsets (Work Coordinate System Select), (G53)
Format:
G53 Oxx Xn Yn Zn Un Wn C
Use the work coordinate system (G53), commonly known as fixture
offsets, to shift Absolute Zero to a preset dimension. G53 dimensions
are referenced to Machine Zero.
G53 cancels Mirror Image (M100), Axis Rotation (G68) and Scaling
(G72).
99 offsets (zero shifts) are available. Offsets are stored in a table. To
activate the Fixture Offset Table in Manual Mode, press F9 (Tool) + F1
(Offsets). You can update this table through the program. If you use a
G53 command to change the offsets in the table, the CNC will overwrite
the values in the Fixture Offset Table.
The letter O followed by the Fixture Offset Table number (1 to 99) defines
an offset.
Fixture Offset Table
The Fixture Offset Table, accessed via the Manual screen, contains the
entered values for Fixture Offsets 1 to 99.
Activating the Fixture Offset Table
To activate the Fixture Offset Table:
1. In Manual Mode, press F9 (Tool) + F1 (Offsets). The Fixture Offset
Table activates. Refer to Figure 4-10.
Figure 4-10, Fixture Offset Table
All rights reserved. Subject to change without notice.
17-April-04
4-17
CNC Programming and Operations Manual
P/N 70000487G - Preparatory Functions: G-Codes
Changing Fixture Offsets in the Table
To change a fixture offset to a manually entered coordinate:
1. Highlight a Fixture Offset (row 1 to 99) in the Fixture Offset Table.
2. Press an axis key (X, Y, or Z).
3. Type a value. Press ENTER. The CNC stores the value in the table.
Adjusting Fixture Offsets in the Table
To adjust an existing fixture offset:
1. Highlight a Fixture Offset (row 1 to 99) in the Fixture Offset Table.
2. Press the letter A key to display the message, “Enter axis and
adjustment value.”
3. Type the axis to adjust (X, Y, or Z) and the amount of the adjustment.
The adjustment value may be positive or negative.
4. Press ENTER to adjust the value, and display the adjusted value in the
table.
Changing Fixture Offsets Using Calibrate Soft Keys
To change a fixture offset using the Calibrate soft keys, CalibX (F5),
CalibY (F6), or CalibZ (F7):
1. Move the machine table to the desired zero position (using a manual
move, jog, handwheel, or MDI).
2. Press the arrow key to highlight the fixture offset in the Fixture Offset
Table.
3. Press the Calibrate soft key(s) for the desired coordinate(s).
G53 Programming Examples
G53 examples #1 to #3 below will clear any active G92.
1. Use offset number three from preset table: G53 O3
Activates a zero point previously entered in the table.
2. Clear any active offset: G53 O0
Use to clear any offset of G53 or G92. It resets the current zero to
Machine Home.
3. Update offset table, shift coordinates: G53 On Xn Yn Zn Un C
The C word tells the CNC to update the table. Use as an immediate
command to shift Absolute Zero and save values in the offset table.
4. Update offset table, but do not activate the shift:
G53 On Xn Yn Zn Un
is used when offsets are defined at the beginning of a program. It is
strictly to set up the offset table.
4-18
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Preparatory Functions: G-Codes
G92 can be used in reference to (after) any G53 active, or without any
G53 active (G53 O0). G53 is modal, and G53 O0 (use none) is active at
power-up.
NOTE: Use G40 to cancel G41/G42 before programming G53.
Modal Corner Rounding/Chamfering (G59, G60)
Use G59 to program modal corner rounding or chamfering. The cornerrounding format blends the intersection of two moves. The chamfer
format chamfers the intersection of two moves. You can use G59 at the
intersection of non-tangent line-line, line-arc, arc-line, and arc-arc moves
(provided a blend radius or chamfer is possible). You cannot blend radii
at the intersection of a line tangent to an arc.
G59 can be used to blend inside or outside radii. Tool diameter
compensation can be active during modal corner rounding. When you
blend inside radii with diameter compensation active, the blend radius
must be greater than the tool radius.
R defines the radius value for corner rounding. E defines a chamfer size.
Refer to Table 4-15. G59 is modal. It will stay active until canceled with
a G60 code. The CNC activates linear interpolation (G1) with G59. You
do not have to program G01 prior to the G59 block.
Corner Rounding Format: G59 Rn
Chamfer Format:
G59 En
Cancel G59:
G60 (Cancels G59 immediately.)
Cancel G59:
G60 Xn Yn Zn (Cancels G59 after move.)
Table 4-15, G59 Address Words
Address Word
R
E
Description
Corner radius
Chamfer distance
G60 cancels G59 immediately. G60 Xn Yn Zn cancels G59 at the end of
the move it contains (as in N13). For example, if G60 were programmed
on a block prior to the X0 move, the lower-left corner would not be
rounded.
You can change the blend radii or chamfer value between moves. To
change the radius to .25 for the bottom two corners, insert G59 R.25
between Blocks N10 and N11. The new radius would apply on the next
move (after Block N10).
All rights reserved. Subject to change without notice.
17-April-04
4-19
CNC Programming and Operations Manual
P/N 70000487G - Preparatory Functions: G-Codes
In the example in Figure 4-11, G59 is used to command modal corner
rounding. Whenever the CNC encounters an intersection between
line-line, arc-arc, or line-arc moves, it will round off the intersection to the
specified radius.
X0Y0
Dimensions:
3 x 2 IN.
(76.2 X 50.8MM)
R = .375 IN.
(9.53 MM)
G59PROG
Figure 4-11, G59 Programming Example
Table 4-16 describes the required program blocks.
Table 4-16, G59 Programming Example, Inch
Blk. #
4-20
Block
N4
N5
N6
N7
N8
N9
N10
N11
N12
N13
G17 G90
G0 X-.5 Y-.5
Z-.25
G1 X0 F20
G59 R.375
Y0
X3
Y-2
X0
G60 Y.5
N14
G0 Z.1
Description
* Set plane and absolute
* Move to point
* Lower Z-axis
* Move to X0 and set feedrate
* Set G59 and radius value
* Move to Y0
* Move to X3
* Move
* Move
* Move to Y.5, then deactivate modal corner
rounding
* Raise Z-axis
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Preparatory Functions: G-Codes
In-Position Mode (Exact Stop Check) (G61)
While the In-Position Mode (G61) is active, the CNC approaches target
and performs an in-position check before the next move is executed.
Refer to Table 4-17. The CNC comes to a complete stop at the
completion of each command. This could cause tool dwell marks to
appear on the work, but prevents the CNC from rounding off sharp
corners.
Table 4-17, G61 and Associated G-Code Formats
Code
Format
G9
G9 Xx.x Yx.x
G61
G61 Xx.x Yx.x
G64
G64
Action
Activates Non-modal In-Position Mode.
Complete stop only in this block.
Activates Modal In-Position Mode. CNC
stops to verify location of each endpoint.
Cancels G61 and activates the Contouring
Mode (Continuous Path Mode).
NOTE: Rapid moves are always performed in In-Position Mode.
G61 is modal and remains in effect until canceled. Use Contouring Mode
(G64) to cancel the G61. Non-modal In-Position Mode (G9) remains
active only for a single block.
NOTE: The In-Position and Continuous Path Tolerances are defined in
the Setup Utility. The In-Position Tolerance should be closer to
target than the Continuous Path Tolerance.
Automatic Feedrate Override for Arcs (G62, G63)
G62 commands an automatic feedrate override for arcs. It slows down or
speeds up the programmed feedrate, based on the cutter compensation
code active (G41 or G42) the tool type and the arc radius. G62 keeps
the edge of the tool that contacts the work cutting at the programmed
feedrate.
Format:
G62
Cancel Format: G63
Example:
NOTE:
While milling a 90-degree CCW inside corner using
G41, the feedrate is overridden (slowed down), in order
to keep the cutting edge of the tool moving at the
programmed feedrate. The opposite would apply on
an outside corner using G42.
You can default this feature to ON or OFF using the Setup
Utility.
All rights reserved. Subject to change without notice.
17-April-04
4-21
CNC Programming and Operations Manual
P/N 70000487G - Preparatory Functions: G-Codes
Contouring Mode (Cutting Mode) (G64)
The Contouring Mode (G64), also known as Continuous Path Mode or
Cutting Mode, is active at power on. Refer to Table 4-18. It is used for
feed moves. With the Contouring Mode activated, the CNC approaches
target and comes within the Continuous Path Tolerance of the target
position. No in-position check is made before the next move is executed.
This enables the smooth contouring of a profile or surface.
Format:
G64
Table 4-18, G64 and Associated G-Code Formats
Code
Format
G9
G9 Xx.x Yx.x
G61
G61 Xx.x Yx.x
G64
G64
Action
Activates Non-modal In-Position Mode.
Complete stop only in this block.
Activates Modal In-Position Mode. CNC
stops to verify location of each endpoint.
Cancels G61 and activates the Contouring
Mode (Continuous Path Mode).
NOTE: Rapid moves are always performed in In-Position Mode.
NOTE: the machine builder defines The In-Position and Continuous
Path Tolerances in the Setup Utility.
G64 is modal and remains in effect until canceled. Use Exact Stop
Check (G61) to cancel the Contouring Mode. G64 initiates linear
interpolation (G1).
User Macros (G65, G66, G67)
NOTE: Before using macros, you must understand how variables and
parameters are used in a program or subprogram. Refer to
“Section 19 - Advanced Programming Features” for an
explanation of these features.
NOTE: G65 or G66 codes always contain some letter variable(s) (Pn,
An, Bn, etc.) to be passed to the macro (subprogram).
4-22
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Preparatory Functions: G-Codes
A macro is a group of instructions stored in memory and called by the
main program when needed. Think of macros as sophisticated, flexible
subprograms, which can be modal (G66) or Non-modal (G65). Refer to
Table 4-19.
Macros might consist of:
q Customized canned cycles to simplify the programming of a particular
part or entire programs for similar part production.
q Parameters (Pn, An, Bn, etc.) passed to the subprogram by letter
address, similar to canned cycles.
q Automatic measuring sequences using sensors, such as probes, for
feedback to the CNC.
Table 4-19, Macro G-Codes
Format
G65 Pn Ln
G65 Pn
G65 Pn, An,
Bn, etc.
M/NM
Non-modal
G66 Pn
G66 Pn, An,
Bn, etc
Modal
G67
Cancel
Action
Executes Non-modal Macro (Pn), with
optional repeat loop, at current location.
Macro is repeated number of times
specified in command (Ln). If the L
address word is omitted, the macro will be
executed only once.
Pn = macro number (O).
Ln = optional loop. Specify number of
times the macro should repeat (n).
Executes called macro (Pn) after each
programmed move until canceled with a
G67 command.
Pn = called macro.
Cancels Modal Macro (G66).
Table 4-20 lists and describes the Address Words and M-codes used
with macros.
Table 4-20, Macro Address Words
Address Word
Format
Pn
Pxxxx
Ln
Lxxxx
On
N(block
Number) Oxxxx
M99
M99
Description
Used in G65 and G66 commands.
Lists macro number (O) to be called.
Used only in G66. Optional repeat
command. Specify number of times
macro should repeat (1 to 9999).
Macro number that occurs in the first
line of the macro; for identification.
End macro (subprogram) and return
to line following G65 or G66 in main
program.
A subprogram consists of fixed dimensions, but a macro contains
variables and parameters that can change every time the macro is used.
The CNC can pass values to variables in the G65 or G66 command.
All rights reserved. Subject to change without notice.
17-April-04
4-23
CNC Programming and Operations Manual
P/N 70000487G - Preparatory Functions: G-Codes
Macros can be stored in the same file as the main program or in a
separate file. Use the File Inclusion feature to call Macros stored in a
separate file.
Refer to “Section 19 - Advanced Programming Features” for a more
detailed explanation of Parameter Passing and Variables and File
Inclusion.
Macros stored in the same file as the main program are defined in the
same way as a subprogram; with the O address word followed by a label
number. The macro is terminated with the M99 code and entered into
the Program Listing after the main program. Refer to Table 4-21.
If the command contains an L address word, the macro is repeated the
specified number of times before the CNC returns to the main program.
Table 4-21, Macro Program List
Program Block
N200 M2
N210 O201
N220 [Enter macro here]
N230
N240
N250
N260 M99
Description
End main program
Macro number assigned
Macro program
End macro, return to next line of main
program. The CNC returns to the line
following the Macro call (G65 or G66) in
the main program.
Use the G65 Macro call to call a macro into the main body of the
program. Refer to Table 4-22.
Table 4-22, Macro Call in Main Program
Program Block
N40
N50 G65 P201
N60
Description
CNC executes Macro O201 once, at
present location.
After executing the macro (M99
encountered), the CNC returns to the
main program and performs the next
programmed command.
The CNC executes the macro (201) at block 50, with or without repeated
loops, as programmed. When the CNC detects the M99 (End Macro)
Code, it returns to the next line of the main program (N60).
4-24
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Preparatory Functions: G-Codes
Axis Rotation (G68)
G68 is modal and remains active until canceled. Refer to Table 4-23.
The CNC automatically cancels rotation if you program S and L. Use
only the listed codes.
Activate Format:
G68 In Jn Sn Cn Pn Ln
Cancel Format:
G68
Table 4-23, G68 Address Words
Address Word
Description
I
J
S
Center of rotation (polar origin) in X-axis. Optional.
Center of rotation (polar origin) in Y-axis. Optional.
Start angle (referenced original programmed
angular position). This variable is used only if L and
P are programmed. Optional.
Angle of Rotation. Required.
Subprogram number to call. Optional.
Number of loops. Number of times C will increment,
and subprogram P will be called. Optional
C
P
L
Patterns commanded by the program can be rotated using polar
coordinates. Any angle can be described as positive or negative,
depending on how it is referenced. CCW from 0 degrees is positive. CW
from 0 degrees is negative. Refer to Figure 4-12.
Figure 4-12, G68 Angle Rotation Guide
All rights reserved. Subject to change without notice.
17-April-04
4-25
CNC Programming and Operations Manual
P/N 70000487G - Preparatory Functions: G-Codes
Minimum data entry for G68 rotation is: G68 Cn. If I and J are not given,
the current position is used. S angle is referenced to the original
programmed position. For example: If a slot is programmed at the 90degree position, S is referenced from 90 degrees. S should be used only
if L and P are programmed. C must be programmed. P and L are
optional. They enable a loop to be executed, so the subprogram will be
called at each angle increment. G17, G18, or G19 must be commanded
prior to programming G68.
G68 Programming Examples
Example 1:
Refer to Figure 4-13 and Table 4-24.
X38.1, Y.5
(X1.5, Y12.7mm)
30 deg.
0
X0Y0
Polar Origin
Figure 4-13, G68 Programming Example 1
Table 4-24, G68 Programming Example 1
Blk. #
Block
N21
G17 G90
N22
G68 I1.5 J.5 C30
N23
M98 P1001
N24
G68
Required Subprogram:
O1001
G90 G0 X2.5 Y.375
G1 Z-.125 F5
X3.5
G3 Y.625 J.125
G1 X2.5
G3 Y.375 J-.125
G0 Z.1
M99
Description
* Set plane and absolute
* Activate rotation to values
* Execute subprogram
* Cancel rotation
Example 1 does not use S, C, P, or L. (No loop is required.)
N21 sets the XY plane and Absolute Mode. N22 enables rotation angle
of 30 degrees, the origin is X1.5 Y.5. N23 executes sub 1001 at the
rotated position. The sub is programmed at the 3 o'clock position. N24
cancels polar rotation.
4-26
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Preparatory Functions: G-Codes
Example 2:
Refer to Figure 4-14 and Table 4-25.
Figure 4-14, G68 Programming Example 2
Table 4-25, G68 Programming Example 2
Blk. #
N1
N2
N3
N4
N5
N6
N7
N8
N9
N10
N11
N12
N13
N14
N15
N16
N17
N18
N19
N20
Block
O688 * G68-2
G90 G70 G17 G0 T0 Z0
X0 Y0
T1 * .25 MILL
Y2.5 Z.1
G1 Z-.125 F5
G41 Y1.875 F14
G68 I0 J0 S0 C-45 P1 L8
G40 G90 G1 Y2.5
G0 T0 Z0
X0 Y0
M2
O1 * 45 DEG. SECTION
G91 G2 X.3542 Y-.4981 I0 J-.375
G3 X.3689 Y-.1528 I.1889 J-.0656
G2 X.6027 Y.1017 I.3376 J-.1634
M99
Example 2 uses all variable words of the G68 function. Only the path
from the 12 o'clock position (90 deg.) to the 1:30 position (45 deg.) is
programmed in the subprogram. The G68 loop increments the angle and
recalls the subprogram to complete the shape.
N1 through N4 set program number, modals, position and tool activation.
N5 and N6 move the tool to the starting position.
All rights reserved. Subject to change without notice.
17-April-04
4-27
CNC Programming and Operations Manual
P/N 70000487G - Preparatory Functions: G-Codes
N7 initiates tool compensation during a move to the 12 o'clock position.
N8 calls the G68 rotation function: origin (I,J) at X0 Y0, starting angle (S)
of zero degrees (First call of subprogram will not be rotated), angle
increment (C) of -45 deg. (CW is negative), call subprogram (P) 1, and
loop count (L) equals eight.
N9 Cancels compensation during the move back to the starting position.
N10 to N12 cancel tool, move to position and end the program.
N16 to N20 define the 45-degree section for the shape, from 12 o'clock
position to 1:30 position.
NOTE:
If you are using S and L format, you do not need to cancel G68.
NOTE:
Select the plane prior to G68 (default is G17). Program
dimensions for both axes of the active plane.
The CNC interprets IJKABC values in the current Absolute/Incremental
Mode. If C is absolute, the 3 o'clock position is 0 degrees. If C is
incremental (G91), the current angle is 0 degrees. It is better to use
incremental (G91) dimensions.
Activating Inch (G70) or MM (G71) Mode
Inch Mode Format: G70
MM Mode Format:
G71
Change the unit of measurement displayed by the CNC by using Inch
Mode (G70) or MM Mode (G71). Refer to Table 4-26. The Inch/MM
Mode is usually specified at the start of a program.
Table 4-26, Activating the Inch/MM Mode
Block
Format
Description
N2
G70 G90 G0
Activates Inch Mode.
N2
G71 G90 G0
Activates MM Mode.
NOTE: The display resolution (number of decimal places shown) is set
up in the Setup Utility. The default resolution is four decimal
places for Inch Mode; three decimal places for MM Mode.
4-28
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Preparatory Functions: G-Codes
Axis Scaling (G72)
Use Axis Scaling (G72) to enlarge or reduce patterns commanded by the
program. Refer to Table 4-27. G72 is modal. If a variable word is not
given, it is assumed to be x1 factor. Axes for circular motion must have
the same factor. .
Activating Format: G72 Xn Yn Zn Un
Table 4-27, Cancel Format: G72
Address Word
X
Y
Z
U
Description
Scaling factor for X-axis
Scaling factor for Y-axis
Scaling factor for Z-axis
Scaling factor for U-axis
Tool length offsets, diameter offsets, tool wear factors, and cutter
compensation are not affected by G72. No other codes are allowed on a
G72 block.
WARNING:
Never program a T-code (T0, T1) while in G72.
Activate the Tn command before G72, then deactivate G72 before
deactivating the Tn command. This applies to all tools (T0 to T99).
Example:
G72 X2 Y2 Z1
The CNC will scale all X and Y moves to twice their programmed size. Z
moves will not be scaled (times 1). Z could have been omitted.
Activating Absolute (G90) or Incremental (G91) Mode
You can change the program mode to G90 or G91. Specify Absolute or
Incremental Mode at the start of a program. Refer to Table 4-28.
Absolute Mode Format:
G90
Incremental Mode Format: G91
Table 4-28, Activating the Absolute/Incremental Mode
Block
N2
N2
Format
G70 G90 G0
G70 G91 G0
All rights reserved. Subject to change without notice.
17-April-04
Description
Activates the Absolute Mode
Activates the Incremental Mode
4-29
CNC Programming and Operations Manual
P/N 70000487G - Preparatory Functions: G-Codes
Absolute Zero Point Programming (G92)
The G92 code is used to set axes to zero (reset) or to new coordinates
(preset). It is sometimes used to set Part Zero. You can use G92 to set
Part Zero on a vise or a fixture. Anilam recommends using G53 (Fixture
Offset) instead of G92.
G92 cancels Mirror Image (M100), Axis Rotation (G68), and Axis Scaling
(G72).
Feed in IPM (G94)
Feedrates for Inch Mode (G70) are programmed as inch/minute (IPM).
F1 = 1.0 IPM
Feedrates for Metric Mode (G71) in mm/min. F1 = 1 mm/min
There are several ways to determine the feedrate. One method is to
multiply (RPM of the cutter) times (feed per revolution).
Example:
A four-flute .7500" endmill is used to finish mild steel at 508 RPM. The
feed per tooth (fpt) is .003". fpt x #t x RPM = in/min
.003 x 4 x 508 = 6.1 in/min (approx.)
Program the feedrate at 6.1 in/min.
If the machine has a rotary axis, give the feed in degrees per minute
(dpm), whether for Inch Mode (G70) or Metric Mode (G71).
6000M-4X
6400M
FU1 = 1 dpm
4-30
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Preparatory Functions: G-Codes
Feed Per Revolution (G95)
Format:
G95 F.0080
feed .0080" per revolution if in G70 (inch) mode.
G95 F.02
feed .02 mm per revolution if in G71 (mm) mode.
If you use feed per revolution (G95), your machine must be equipped with
an encoder on the spindle for feedback.
The calculated rate in in/min or mm/min must not exceed the maximum
feedrate allowed.
Adjusting Feedrate
You can run the CNC at a percentage of the programmed feedrate by
adjusting the FEEDRATE OVERRIDE switch. Each click of the FEEDRATE
OVERRIDE switch adjusts the feedrate by an increment of ten percent; the
range is 0 to 120%. Set FEEDRATE OVERRIDE to 100 to set the feedrate to
100% of the programmed feedrate.
CAUTION: If the CNC is shut down, the setup file will reload a
default feedrate at the next power-on.
All rights reserved. Subject to change without notice.
17-April-04
4-31
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Section 5 - Ellipses, Spirals, Canned Cycles, and Subprograms
Ellipses (G5)
Format: G5 Xn Yn In Jn An Bn Ln
Use G5 to program a full or partial ellipse. You must know the following
variables and program them after the G5 code. Refer to Table 5-1 and
Figure 5-1.
Program the starting point prior to G5. It must lie along the ellipse.
Table 5-1, G5 Address Words
Address
Word
Description
X
Incremental X end point (or distance from start to end)
Y
Incremental Y end point (or distance from start to end)
I
Incremental X center point (or distance from start to center)
J
Incremental Y center point (or distance from start to center)
A
Half-length of ellipse in X-axis *
B
Half-width of ellipse in Y-axis *
Direction of tool travel: 1 is CCW; -1 is CW
L
*Half-length is the dimension of a quadrant of the ellipse. For a full
ellipse, it is half the X length (for A variable), and half the Y width (for B
variable). A and B are always positive.
2
1
ELLIPSE
Figure 5-1, Ellipse Programming Example
All rights reserved. Subject to change without notice.
17-April-04
5-1
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
G5 X0 Y0 I2 J0 A2 B1 L-1
The block will cut a full CW ellipse, 4 x 2 in size, beginning at X0 Y0, in
Absolute Mode (G90).
NOTE:
G5 is plane dependent (word groups: XYZ, IJK, AB, L).
G41 and G42 are not allowed with G5. However, you can compensate
ellipses by programming a special variable. This variable is #1040. Set
#1040 to one of the following values:
#1040 = 0 : Sets the ellipse compensation to OFF.
#1040 = 1 : Sets the ellipse compensation to ON, OUTSIDE.
#1040 = 2 : Sets the ellipse compensation to ON, INSIDE.
You must offset the tool from the edge of the ellipse (by the amount of
the tool radius). The ellipse values (length, width, etc.) should be
programmed as if the centerline of the tool is directly over the edge of the
ellipse (value of uncompensated ellipse should be programmed).
#1040 remains active at the programmed value. You do not have to
program it more than once to compensate more than one ellipse.
5-2
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Spiral (G6)
Format: G6 Xn Yn Zn In Jn Ln
Use G6 to cut a spiral. Certain variables must accompany the G-code.
You cannot use Cutter compensation (G40 to G42) with G6. Refer to
Table 5-2.
Table 5-2, G6 Address Words
Address
Word
Description
X
Incremental X end point (or distance from start to end if G91)
Y
Incremental Y end point (or distance from start to end if G91)
Z
Incremental Z end point (or distance from start to end if G91)
I
Incremental X center point (or distance from start to center if
G91)
Incremental Y center point (or distance from start to center if
G91)
Number of complete revolutions and direction of tool travel:
+ is CCW; - is CW
J
L
NOTE: Do not use a spiral to cut a tapered bore.
NOTE: XYIJ values define the center of the spiral. Z defines the Z
depth. These values are Absolute or Incremental as configured
in the Setup Utility under the Circle centers parameter. The
default is Incremental. ANILAM recommends that you do not
change this parameter. Refer to the Setup Utility manual for
details.
The tool start position is the 'counting' position for the number of
revolutions. Example: If a spiral does not make a complete revolution,
L = -.1 or .1. For a spiral that makes ten complete revolutions,
L = 10 or -10. For a spiral that makes six and one half turns, L = 6 or -6.
This block will cut a CCW spiral 1 in. deep, using five revolutions, starting
at X1.5 Y0, using Absolute (G90) Mode. Refer to Figure 5-2, XY View
Spiral and Figure 5-3, Isometric View Spiral.
The spiral will not work into a radius of 0, nor will it start with a radius of 0;
.001" (.01mm) is the minimum radius.
G6 is plane dependent (word groups: XYZ, IJK, L).
Example:
G0 X1.5 Y0 Z0
G6 X-.5 Y0 Z-1 I-1.5 J0 L5
All rights reserved. Subject to change without notice.
17-April-04
5-3
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Y
X1
X1.5
XO,YO
Figure 5-2, XY View Spiral
Y
Z
X
SPIRAL2
Figure 5-3, Isometric View Spiral
Canned Cycles
A canned cycle is a preset sequence of events initiated by a single block
of data. Canned cycles are part of the CNC software and cannot be
altered. They simplify the programming of complicated cycles. One
block of data can instruct the CNC to perform the necessary moves to
drill a hole, mill a pocket, or cut a spiral or ellipse.
A canned cycle consists of a G-Code and variable words. The variable
words describe parameters, such as peck distance, retract height, pocket
depth and tool stepover. Each canned cycle has its own set of variable
words.
The variable words in a canned cycle allow you to customize the cycle to
include the necessary dimensions, feedrates, etc.
5-4
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Canned cycles greatly reduce program blocks. Use them whenever
applicable.
Canned cycles are usually entered into the part program from the Main
Edit Help Menu. Edit Help contains graphics and labeled entry fields to
make programming canned cycles quick and easy. Refer to
“Section 7 - Edit Help” for details.
Drilling, Tapping, and Boring Canned Cycles (G81 to G89)
When you activate a drilling cycle, it executes after each programmed
position, until you cancel it.
NOTE: The P entry (return height) is optional, and you do not need to
provide it. If you do not specify P, the CNC will set it to R.
Keep the following in mind for drill cycles:
q
P dimension is optional. If it is not given, the retract height will be the
same as the Z start height (R dimension).
q
F feedrate is optional. If it is not given, the current feedrate is used.
q
All start and finish heights (R and P) as well as Z dimensions are
absolute dimensions.
q
P must be less than R, or an alarm will be given.
q
For all peck drill cycles (G83 and G87), R (start height) must be 0.1"
(or 2 mm) above the work surface.
q
G84 (Tapping) uses S word for Spindle Yes/No. Your machine must
be equipped with spindle M-functions to use G84.
q
Z-axis depth can be changed by placing a new Z depth on the same
line as the X- and/or Y-axis location of the hole you want the new
depth applied. A Z address on a line of its own will cause the control
to drill the new depth at the current location.
All rights reserved. Subject to change without notice.
17-April-04
5-5
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Cancel Drill, Tap, or Bore Cycle (G80)
Format: G80
Modal cycles remain active until canceled. Use G80 to cancel drill, tap,
and bore canned cycles (G81 to G89). G80 can be included with other
commands on a block.
Spot Drilling (G81)
Format: G81 Zn Rn Fn Pn
G81 is a spot drilling cycle, generally used for center drilling or hole
drilling that does not require a pecking motion. It feeds from the start
height (R) to the specified hole depth (Z) at a given feedrate (F), then
rapids to the return height (P). Refer to Table 5-3.
Table 5-3, G81 Address Words
Address
Word
Description
Z
Absolute hole depth. Required.
R
Initial Z start point, in rapid. Required.
F
Feedrate.
P
Z return point after hole depth, in rapid. P must be higher
than R.
Counterboring (G82)
Format: G82 Zn Rn Fn Dn Pn
G82 is the counter bore cycle, generally used for counterboring. It feeds
from the R-plane to Z depth, dwells for specified time, then rapids to the
return point. Refer to Table 5-4.
Table 5-4, G82 Address Words
Address
Word
Z
R
F
D
P
5-6
Description
Absolute hole depth. Required.
Initial Z start point, in rapid. Required.
Feedrate
Dwell time (in seconds). Required.
Z return point after hole depth, in rapid. P must be higher
than R.
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Peck Drilling (G83)
Format: G83 Zn Rn Fn In Pn
G83 is the peck drilling cycle, generally used for peck drilling relatively
shallow holes. G83 feeds from the R-plane to the first peck depth
(calculated so that all pecks are equal and do not exceed the maximum
peck distance programmed in I word). Then rapid retracts to R-plane (to
clear chip), rapids down to previous depth less .02", and continues this
loop until it reaches the final hole depth. It then rapid retracts to the P
dimension. Refer to Table 5-5.
Table 5-5, G83 Address Words
Address
Word
Z
R
F
I
P
Description
Absolute whole depth. Required.
Initial Z start point, in rapid. Required.
Feedrate.
Maximum peck distance (positive dimension). Required.
Z return point after hole depth, in rapid. P must be higher
than R.
All rights reserved. Subject to change without notice.
17-April-04
5-7
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Tapping (G84)
Format: G84 Zn Rn Fn Sn Pn
NOTE: The machine must be equipped with spindle M-functions (FWD,
REV, OFF) to use this cycle. Do not use G84 if the machine
does not have spindle commands available.
G84 is the tapping canned cycle, used for tapping holes. During a G84
cycle: the tool feeds from the R-plane to Z depth; the spindle stops and
reverses; the tool feeds to the retract plane; and the spindle stops and
reverses again. Refer to Table 5-6.
F (TPI/Lead): Enter Threads Per Inch when in Inch mode. Enter Lead
when in MM (G71) mode. Lead is the distance from one thread to the
next. You must program a spindle RPM. The Feedrate is calculated
based on the spindle RPM and the TPI or Lead specified.
S (Spindle sync): To enable Spindle sync, enter a value of 1. The
machine must have direct spindle control to use this feature. The spindle
rotation and Z-axis movement will be synched together, as in a threading
cycle.
D (Dwell): A dwell time value in seconds can be entered. You may
require this feature because of the time required to stop and reverse the
spindle.
NOTE: If S=0, the programmed Dwell (D) will be active when the
spindle reverses at the bottom and top of each hole.
If S=1, the programmed Dwell (D) will be at the top of each hole.
Table 5-6, G84 Address Words
Address
Word
5-8
Description
Z
Absolute hole depth. Required.
R
Initial Z start point, in rapid. Required.
F
S
Threads per Inch (TPI) in Inch mode, or
Lead (Distance between threads) in MM mode.
Spindle, No (0), or Yes (1).
P
Z retract height after hole depth, in feed.
D
Dwell time.
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Boring, Bi-directional (G85)
Format: G85 Zn Rn Fn Pn
G85 is a boring cycle, generally used to make a pass in each direction on
a bore or to tap with a self-reversing tapping head. It feeds from the
R-plane to Z depth, and then feeds back to the retract height. Refer to
Table 5-7.
Table 5-7, G85 Address Words
Address
Word
Description
Z
Absolute hole depth. Required.
R
Initial Z start point, in rapid. Required.
F
Feedrate.
P
Z return point after hole depth, in feed.
Boring, Unidirectional (G86)
Format: G86 Zn Rn Fn In Dn Pn Cn
G86 is a boring cycle that allows the X-axis to back off the bore surface
after the spindle has stopped and oriented itself. The cycle will feed from
the R-plane to Z depth, dwell for the specified time, stop and orient the
spindle to the specified angle C, back off in X, rapid retract in Z, reposition in X, and restart the spindle. Refer to Table 5-8.
NOTE: Your machine must be equipped with spindle M-functions
(FWD, REV, OFF) and spindle orientation (M19) to use this
cycle. Do not use the G86 cycle if the machine does not have
the spindle commands and spindle orientation.
Table 5-8, G86 Address Words
Address
Word
Description
Z
Absolute hole depth. Required.
R
Initial Z start point, in rapid. Required.
F
I
Feedrate.
X-axis incremental backoff distance in X (positive or
negative dimension).
Dwell time (in seconds).
Z return point after hole depth, in rapid.
M19 index angle. If no angle is given, the angle in
MC_5003, Default Spindle Orientation Angle, is used.
D
P
C
All rights reserved. Subject to change without notice.
17-April-04
5-9
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Chip Breaker Peck Cycle (G87)
Format: G87 Zn Rn Fn In Jn Kn Wn Un Pn
G87 is the chip-breaker peck-drilling cycle, generally used to peck-drill
medium to deep holes. The cycle feeds from the R-plane to the first peck
depth in Z, rapid retracts the chip-break increment (W), feeds to the next
calculated peck depth (initial peck less J), and continues this sequence
until it reaches a U depth, or until final hole depth is reached. The peck
distance will never be more than I or less than K. Refer to Table 5-9.
This cycle enables optimum drilling conditions for holes. For maximum
efficiency in deep hole drilling, set parameters to accommodate the
material and tool types used. Generally, the deeper the hole, the smaller
the peck distance (J). This prevents the binding of chips, tool, and
workpiece. Set U to retract the drill completely at set depth intervals.
Table 5-9, G87 Address Words
Address
Word
Z
Absolute hole depth. Required.
R
Initial Z start point, in rapid. Required.
F
Feedrate.
I
First peck distance (positive dimension). Required.
J
K
Amount to subtract from previous peck (positive
dimension). Required.
Minimum peck distance (positive dimension). Required.
W
Chip break increment (positive dimension).
U
Incremental depth between full retracts (positive
dimension).
Z return point after hole depth, in rapid. P must be higher
than R.
P
5-10
Description
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Flat Bottom Bi-Directional Boring (G89)
Format: G89 Zn Rn Fn Dn Pn
G89 is a boring cycle, generally used to program a pass in each direction
with a dwell at the bottom. The tool feeds from the R-plane to Z depth,
dwells for specified time, then feeds to the retract (P) dimension. Refer
to Table 5-10.
Table 5-10, G89 Address Words
Address
Word
Description
Z
Absolute hole depth. Required.
R
Initial Z start point (0.1 inch or 2 mm), in rapid. Required.
F
Feedrate.
D
Dwell time (in seconds). Required.
P
Z return point after hole depth, in feed.
Drilling Example
The following example assumes that the machine has no automatic tool
changer (ATC). If your machine has an ATC, check your machine
manual for proper tool changer programming procedures. Refer to
Figure 5-4 and Table 5-11, Drilling Example, Inch (Metric).
Drilling
Figure 5-4, Drilling Example
All rights reserved. Subject to change without notice.
17-April-04
5-11
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Table 5-11, Drilling Example, Inch (Metric)
Blk #
5-12
Block
N1
O1 * DRIL-X1
N2
G90 G70 (G71) G0 T0 Z0
N3
N4
N5
X-3.0 (X-75) Y1.0 (Y25)
T01 * 1/4" DRILL (6.35 DRILL)
G83 Z-.55 (Z-14) R.1 (R2) F12
(F300) I.08 (I2) P.1 (P2)
N6
N7
N8
X1.0 (X25.4) Y-1.0 (Y-25.4)
X3.0 (X76.2)
G91 X1.5 (X38.1)
N9
N10
N11
N12
X1.0 (X25.4) Y -1.25 (Y-31.75)
X-2.5 (X-63.5)
G90 X1.5 (X38.1) Y -2.5 (Y-63.5)
G80 T0 Z0
N13
N14
X-3.0 (X-75) Y1.0 (Y25)
M02
Description
Program number (1) and name (DRILLEX1).
Sets absolute dimensions (G90), inch
input (G70), rapid (G0), cancel any
active tool (T0), and bring Z to zero (Z0).
Move to X-3 Y1.
Activate Tool #1 length offset.
Initiates peck drill cycle G83: Z = hole
depth, R = start height, F = feedrate, I =
maximum peck, P = return height.
Hole location #1 (Rapid and Absolute).
Hole #2.
Hole #3 (moves from #2 to #3 in
incremental: G91).
Hole #4 (Incremental).
Hole #5 (Incremental).
Hole #6 (Absolute).
Cancel drill cycle (G80), cancel tool
(T0), and rapid Z to zero (Z0).
Move to X-3 Y1 for part change.
End Program.
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Pattern Drill Cycles
Use the automatic bolt hole circle (G79) to drill a partial or full bolt circle.
A drill cycle (G81 to G89) must be programmed prior to G79. You can
move around the pattern clockwise or counterclockwise, either point to
point or along a radius. G79 calculates the hole locations. The cycle
uses the Polar Coordinate System for dimensions. Refer to Table 5-12
and Figure 5-5. When the G79 cycle is completed, you must cancel the
cycle (G80).
Bolt Hole Circle (G79)
Format: G79 Xn Yn Cn An Bn Hn Dn R
Table 5-12, G79 Address Words
Address
Word
X
Y
C
A
B
H
D
R
Description
Absolute X center of the bolt-circle. Defaults to current
position.
Absolute Y center of the bolt-circle. Defaults to current
position.
Rotates the Polar Coordinate System by entered angle.
Default: 0 degrees (3 o'clock). CCW = positive, CW =
negative.
Angle of the first hole. Required.
Angle of the last hole. If there is no B value, the CNC will
execute a full bolt hole circle.
Number of holes in full bolt circle. Required.
Diameter of bolt circle. Tool will normally move from hole to
hole in a CCW (positive) direction. For CW direction, D =
negative. Required.
Move from hole to hole on a radius. Set to 1.0 to activate.
Defaults to point-to-point and hole-to-hole.
POLAR
Figure 5-5, Polar Coordinates
All rights reserved. Subject to change without notice.
17-April-04
5-13
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Hole Pattern (G179)
Format: G179 Xn Yn Cn An Bn Dn En Un Vn Wn
NOTE: Do not program G68 with G179.
Use the automatic hole pattern canned cycle (G179) to program partial or
full pattern hole grids. You can use G179 for a corner pattern when holes
are required only on four corners. It calculates the hole locations from
the entered variables. You can also rotate the pattern around the starting
hole location. A drill cycle (G81–G89) must be programmed prior to
G179. You must cancel the cycle (G80) after the pattern is completed.
Refer to Table 5-13.
You can use [A and D] or [U and V], but not both combinations. Positive
and negative values are allowed in all variable words except: B, E, and
W.
Table 5-13, G179 Address Words
Address
Word
X
Y
C
A
B
D
E
U
V
W
Description
Absolute X position of start hole.
Absolute Y position of start hole.
Angle to rotate the hole pattern. Default is 0 degrees (3
o'clock position).
Length of pattern in X-axis. If used, U cannot be given.
Number of holes in X-axis. Required.
Width of pattern in Y-axis. If used, V cannot be given.
Number of holes in Y-axis. Required.
Increment between holes in X-axis. Can be used instead of
A.
Increment between holes in Y-axis. Can be used instead of
D.
Pattern or Square. If W is 0, then a matrix pattern will be
drilled. If W is 1, then a perimeter pattern (edges only) will
be drilled. Refer to Figure 5-6.
Figure 5-6, Matrix vs. Perimeter Pattern
5-14
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Example:
G81 Z-.1 R.1 F15
G179 X2 Y1 C30 B6 E4 U.5 V.375 W0
G80
These blocks rotate a bolt hole pattern 30 degrees counterclockwise.
Refer to Figure 5-7.
G179
Figure 5-7, G179 Programming Example
All rights reserved. Subject to change without notice.
17-April-04
5-15
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Pocket Cycles
Pocketing cycles eliminate extensive programming. One block of
programming will mill out the described pocket. Activate a tool before
programming a pocket cycle. All pockets use the current tool diameter
from the Tool Page.
XY positioning may be necessary prior to programming a pocket cycle.
Programmer is responsible for all Z moves in Hole Mill (G76) cycle.
Cutting direction is reversible in the pocketing cycles.
Always check that tool-to-corner radii do not conflict.
Z and P dimensions are absolute.
On all cycles with variable A (tool stepover), A must be less than the tool
diameter. In G78 and G178, A must be 70% or less of tool diameter.
Alarm messages will occur if the CNC detects program errors.
G41 and G42 are not permitted during pocket cycles. Pocket cycles use
"built-in" cutter compensation.
Stock variable #1030 is not permitted and will be ignored.
WARNING: When you cut one pocket inside another, make sure to
set P above the highest pocket. At the end of each
pocket, the tool will rapid to P, then rapid to the start
position.
For plunge pockets (G177, G178), drill a start hole prior to activating the
pocket; position the axes over the start hole prior to G177 or G178.
5-16
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Draft Angle Pocket Cycle (G73)
Format: G73 Xn Yn Hn Zn An Bn Cn Dn En In Vn Sn Qn Rn Wn
Use the draft angle pocket cycle (G73) to machine a draft angle on a
pocket. The tool must be at the center point of the lower-left corner
radius. This is where the machining begins. You can use G78 to mill out
an initial pocket prior to the G73 block. Refer to Table 5-14.
Table 5-14, G73 Address Words
Address
Word
X
Y
H
Z
A
B
C
D
E
I
J
V
S
Q
R
W
Description
X length at the bottom of the pocket. Required.
Y width at the bottom of the pocket. Required.
Z absolute rapid start height (must be 0.1 inch or 2 mm
above surface). Required.
Z absolute pocket depth. Required.
Lower-left corner radius. Cannot be less than tool radius.
Required.
Lower-right corner radius. Cannot be less than tool radius.
Optional.
Upper-right corner radius. Cannot be less than tool radius.
Optional.
Upper-left corner radius. Cannot be less than tool radius.
Optional.
Draft angle to be machined on vertical walls of pocket.
Required.
Z-axis roughing step-down. Required.
Roughing feedrate (does not appear in Help Menu).
Maximum XY tool stepover. Used if angle is so great that
the amount of XY step per Z step exceeds 70 % of the tool
diameter. Optional.
XY finish stock amount, sides only. Optional.
Z-axis finishing step-down. Optional.
Finish-pass feedrate. Optional.
Flat end mill = 0. Ball end mill = 1. Optional. Default is flat
end mill.
All rights reserved. Subject to change without notice.
17-April-04
5-17
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Example:
This program will cut the draft pocket shown in the figure. The drawing
does not show the finish pass. Assume an existing rectangular pocket (4
in. long x 2 in. wide x 1 in. deep) with a theoretical sharp lower-left corner
at X2 Y2. The following program will machine a draft angle onto the
existing pocket. Refer to Figure 5-8 and Table 5-15.
Figure 5-8, G73 Programming Example
Table 5-15, G73 Programming Example
T1 M3 S2000 ***** 1/2" FLAT END MILL
G90 G0 X2.5 Y2.5 F30 ***** 4" x 2" x 1" DP RCT. PKT ALREADY
EXISTS
G73 X4 Y2 H.1 Z-1 A.5 E10 I.1 S.01 Q.02 R35
G0 T0 Z0 M5
X0 Y0 M2
Position the tool above the center of the lower-left corner radius. The tool
path starts and ends at the center of the lower-left corner radius (after
each perimeter pass) for all roughing passes. During finish passes, the
tool will step down the draft angle and make passes around the
perimeter.
If a ball-end mill is programmed (W=1), the following points must be
considered: If W=1, the length (X) and width (Y) at the bottom of the
pocket is measured at the tangency point of the ball radius and the draft
angle. If W=1, the start height (H) must be set to (.1 + ball radius) above
surface to be cut. If W=1, set the tool-length offset so that the ball is
buried up to its centerline when at the part surface (touch off the tip and
add the ball radius, or touch off tip and use a negative length wear equal
to the ball radius).
5-18
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Frame Pocket Milling (G75)
Format: G75 Xn Yn Mn Wn Hn Zn An Bn In Jn Un Vn Cn Sn Kn Pn
Frame milling (G75) will mill a frame or trough around an island of
material. You must position the XY axes at the lower-left (theoretical
sharp) corner of the island before you program G75. Refer to Table 5-16.
Prior to G75, activate a tool so that the CNC will consider the tool
diameter. The relation of the outside corner radius to the frame width
must be geometrically possible or an Error Message will appear.
Table 5-16, G75 Address Words
Address
Word
X
Y
M
W
H
Z
A
B
I
J
U
V
C
S
K
P
Description
Center of island in X-axis. Default: Current position.
Center of island in Y-axis. Default: Current position.
Length of island in X-axis. Required.
Width of island in Y-axis. Required.
Z absolute starting (rapid) height (must be 0.1 inch or 2 mm
above surface to be cut into). Required.
Absolute depth of frame. Required.
Maximum tool stepover (must be less than tool diameter). +A
dimension = climb (CCW). -A dimension = conventional (CW).
Defaults to half tool diameter.
Maximum Z depth per pass (For example, if Z is programmed to
be -1, and B to be .5, the frame will be roughed out in two levels.)
B is programmed as a positive dimension. Defaults to tool
diameter (depth) less finish stock.
Ramp in feed: The tool will ramp into the first depth of cut with a
YZ move from the I.D. of the frame to the O.D. of the frame.
Defaults to last programmed feedrate.
After the ramp-in move described above, the tool will rough-mill
the frame, at feedrate J. Defaults to last programmed feedrate.
Inside corner radius of frame (corner radius of island). Required.
Outside corner radius of frame. Defaults to value of U. Must be
equal to or greater than tool radius.
Frame width. Required.
Finish stock amount per side (including bottom). If you enter a
negative value, stock will be left, but no finish pass will occur. If
you do not enter a value, finish stock will not be left.
Finish-pass feedrate. Defaults to last programmed feedrate.
Z-axis absolute (rapid) retract height (must be equal to or above
H). Defaults to H value.
All rights reserved. Subject to change without notice.
17-April-04
5-19
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Example:
G75 M3 W1.125 H.1 Z-.375 A.25 B.36 I5 J18 U.25 V.5 C1 S.015 K30 P.1
Figure 5-9 illustrates the moves output by the CNC to mill the frame.
Figure 5-9, G75 Programming Example
The tool will perform the following operations:
NOTE: If X and Y are not provided, position the tool at the center of the
island prior to G75.
1. Tool will rapid from position 1 to position 2: X is the center of the
inside corner radius (U), and Y is the corner radius plus tool radius
plus finish stock.
2. Tool will feed -.1 (or 2 mm) in Z to the part surface.
3. Tool performs a ramp-in move to O.D. of frame minus tool radius
minus finish stock (position 3).
4. Tool then moves 360 degrees CCW around frame back to position 3.
5. Tool then steps over calculated amount, and mills CW until position 2
is reached again at depth.
6. Tool then mills 360 degrees CW (climb-milling) around the island.
NOTE: The number of times the tool repeats Steps 3 through 6
depends on the Z and B dimensions.
7. When the frame is completed, the tool rapids first to the P dimension,
then to the center of the island.
5-20
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Hole Milling (G76)
Format: G76 Xn Yn Dn Zn Bn Hn Sn Jn Kn
Use the hole milling cycle (G76) to machine through holes or counterbores. You can position the tool at the hole center prior to the G76 block.
Activate a tool prior to G76 so that the CNC knows the tool diameter.
Refer to Table 5-17.
If you do not provide Z and H, program a separate Z move to raise the
tool out of the hole after the cycle.
Table 5-17, G76 Address Words
Address
Word
Description
Z
X coordinate of the center. Default: pocket centers at
present position. Optional.
Y coordinate of the center. If no coordinate is provided,
default is set to present position. Optional.
The absolute depth of the finished pocket. Optional.
B
Z-axis increment used for each pass. Optional.
H
Absolute Z position to which the CNC rapids before feeding
into the workpiece. Optional.
Diameter of hole. Negative D = CW direction. The
direction CCW (climb milling) is reversible:
+D dimension = climb (CCW).
-D dimension = conventional (CW).
Required.
Rough-pass feedrate. Defaults to last programmed
feedrate.
Finish-stock amount per side. If you enter a negative
value, stock will be left, but no finish pass will occur. If you
do not enter a value, no finish stock will be left.
Finish-pass feedrate. Defaults to last programmed
feedrate.
X
Y
D
J
S
K
Example:
G76 D2.5 J12 S.01 K20
In Figure 5-10, G76 Programming Example, the tool will perform the
following operations:
1. Tool moves from position 1 to a position 45 degrees from center, at
half the radius (position 2).
2. Tool then arcs onto the O.D. tangential (CCW) (position 3).
3. Tool mills O.D. CCW (position 4).
All rights reserved. Subject to change without notice.
17-April-04
5-21
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
4. Tool leaves O.D. tangentially to a point 135 degrees from the center
at half the radius. CCW (position 5).
5. Tool returns to center (position 6).
6. If you have programmed a finish pass, the process repeats at the
finish dimensions.
3,4
5
2
1
6
2.5" Dia.
G76
Figure 5-10, G76 Programming Example
5-22
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Circular Pocket Milling (G77)
Format: G77 Xn Yn Hn Zn Dn An Bn In Sn Kn Pn
Use the circular pocket canned cycle (G77) to mill round pockets. You do
not have to place the tool at the center of the pocket, since the cycle has
variable words for X and Y center. If X and Y variable words are not
programmed, the CNC will use the current position as the pocket center.
Refer to Table 5-18.
Activate a tool prior to programming G77 so that the CNC will know the
cutter diameter. You can position the tool at the pocket center and omit
the XY words. By default, the CNC will use the current position as the
pocket center.
Table 5-18, G77 Address Words
Address
Word
Description
X
Center of the pocket in X-axis. Defaults to current position.
Y
Center of the pocket in Y-axis. Defaults to current position.
H
Z absolute starting height (0.1 inch or 2 mm above surface).
Required. Executed in rapid.
Z
Absolute depth of pocket. Required.
D
Diameter of pocket. The direction CCW (climb milling) is
reversible: +D dimension = climb (CCW). -D dimension =
conventional (CW). Required.
A
Maximum tool stepover (must be less than tool diameter). If
+A dimension = outward spiral. If -A dimension = inward
spiral. On inward spirals, the tool moves to O.D. at 0 degrees,
and begins the roughing process there (3 o'clock). Defaults to
tool radius.
B
Maximum Z depth per pass (Example: If Z is programmed to
be -1, and B to be .5, the pocket will be roughed out in two
levels.) B is programmed as a positive dimension. Defaults to
tool diameter (depth), less finish stock.
I
Ramp in/rough feed: The tool will ramp into the first depth of
cut with a spiral move from the I.D. of the pocket to the O.D. of
the pocket. The feedrate for this move is programmed as I.
After the ramp-in move, the tool will rough-mill the pocket, at
feedrate I. Defaults to last programmed feedrate.
S
Finish-stock amount per side (including bottom). If you enter a
negative value, stock will be left, but no finish pass will occur.
If not programmed, no finish stock is left.
Finish-pass feedrate. Defaults to last programmed feedrate.
K
P
Z-axis absolute-retract height (must be equal to or above H).
Executed in rapid. Defaults to H dimension (start height).
All rights reserved. Subject to change without notice.
17-April-04
5-23
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Example:
G77 X2 Y2 H.1 Z-.25 D3 A.35 B.25 I12 S.01 K20 P.1
In Figure 5-11, the tool will perform the following operations:
NOTE: Figure 5-11 shows only the tool path.
1. Tool will move to X2 Y2 (position 1) in current modes: G0/1, G90/91,
G70/71 (position 1).
2. Tool will feed .1 in. (2 mm) down in Z-axis.
3. Tool will move to O.D. (less finish stock) in a 3-axis spiral motion
(position 2).
4. Tool will make a full circle (position 2).
5. Tool then spirals inward to complete the roughing cycle, at the first
level.
6. If you have specified a finish pass, repeat steps 3 through 5 at the
finish feedrate.
7. Tool rapids to P dimension, then to the original XY location.
Figure 5-11, G77 Programming Example
5-24
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Rectangular Pocket Milling (G78)
Format: G78 Xn Yn Hn Zn Un An Bn In Jn Sn Kn Pn
Use the rectangular pocket cycle (G78) to mill square or rectangular
pockets. You must position the tool directly over the center of the pocket
prior to the G78 block, or use the X Y words. Refer to Table 5-19.
Activate a tool prior to programming G78, so cutter diameter is known.
Table 5-19, G78 Address Words
Address
Word
Description
M
X coordinate of the center. Default: pocket centers at present
position. Optional.
Y coordinate of the center. If no coordinate is provided, default
is set to present position. Optional.
Length of pocket in X-axis. Required.
W
Width of pocket in Y-axis. Required.
H
Z absolute starting height (must be 0.1 inch or 2 mm above
surface to be cut). Executed in rapid. Required.
Absolute depth of pocket. Required.
X
Y
Z
U
A
B
I
J
S
K
Actual corner radius of pocket (all four corners will be same).
Must be equal to or greater than tool radius. Defaults to tool
radius.
Maximum tool stepover (must be 70% or less of tool diameter).
+A dimension = climb (CCW). -A dimension = conventional
(CW). Defaults to half tool diameter.
Maximum Z depth per pass (Example: if you program Z to be 1, and B to be .5, the CNC will rough out the pocket in two
levels.) B is programmed as a positive dimension. Defaults to
tool diameter (depth), less finish stock.
Ramp in feed: The tool will ramp into the first depth of cut with
an XYZ move from the centerline of the lower-left radius
toward the center of the pocket. The feedrate for this move is
programmed as I. Defaults to last programmed feedrate.
After the ramp-in move, the tool will rough-mill the pocket, at
feedrate J. Defaults to last programmed feedrate.
Finish stock amount per side (including bottom). If entered as
negative, stock will be left, but no finish pass will occur. If not
programmed, no finish stock is left.
Finish-pass feedrate. Defaults to last programmed feedrate.
(Continued…)
All rights reserved. Subject to change without notice.
17-April-04
5-25
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Table 5-19, G78 Address Words (Continued)
Address
Word
P
Description
Z-axis absolute finish height (must be equal to or above H).
Executed in rapid. Defaults to H value.
WARNING: When you cut a pocket inside another pocket,
you must set P above the highest pocket. At the
end of each pocket, the tool will rapid to P, then
rapid to the start position.
Example:
G78 M4 W2 H.1 Z-.5 U.75 A.35 B.25 I7 J12 S.01 K20 P.1
NOTE: If you do not use X and Y words, you must position the tool at
the center of the pocket before the G78 block.
In Figure 5-12, the tool will perform the following operations:
NOTE: Figure 5-12 shows only the tool path.
1. Tool moves to the center of the radius in the lower-left corner
(position 1).
2. Tool feeds -.1” (2 mm) to meet the part surface.
3. Tool moves in XYZ toward center of pocket (position 2) to the first
roughing depth, at feedrate I.
4. Tool mills out the pocket with straight lines and arcs (if necessary),
using feedrate J, until first level is completed.
5. Tool repeats this process if necessary to achieve full depth (less
finish stock).
6. Optional finish pass is made in the same manner at feedrate K.
7. When the pocket is complete, tool rapids to P, then to the center of
the pocket.
2
1
X
2 X 4 OVERALL
G78
Figure 5-12, G78 Programming Example
5-26
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Area Clearance (Irregular) Pocket Milling (G169)
Format: G169 Wn Xn Yn Hn Zn Cn Dn En An Bn Sn In Jn Kn Pn
Use G169 to mill irregular pockets. You must enter the perimeter of the
shape into a subprogram. The first move in the subprogram must be a
rapid move to the pocket start point (corner, end, or most convenient
location). Do not include parametric programming, tool compensation, or
feedrates in the subprogram, only the exact perimeter of the pocket. Use
only closed shapes. In a closed shape, the start point of the first (rapid)
move and the endpoint of the last move (line or arc) are the same. The
CNC will automatically calculate the moves necessary to clear out the
shape. Islands are not allowed. Refer to Table 5-20.
Table 5-20, G169 Address Words
Address
Words
Description
W
The number of the subprogram that contains the perimeter
of the pocket. Must be a closed shape. Required.
X
The X position from which the stepover cuts will begin.
Must be inside the pocket, including the tool radius.
NOTE: ANILAM recommends that you leave this
parameter blank. (The CNC will pick point.)
Y
The Y position from which the step-over cuts will begin.
Must be inside the pocket, including the tool radius.
NOTE: ANILAM recommends that you leave this
parameter blank. (The CNC will pick point.)
H
The Absolute Z position before beginning to mill the pocket.
This must be 0.1 inch (or 2 mm) above the surface.
Z
The Absolute depth of the pocket.
C
The angle of the cut, in reference to 0 degrees (3-o'clock
position). This is necessary only if the first element of the
profile subroutine is an arc, or if you want to change the
original path automatically output by the CNC. Defaults to
angle of the first subprogram move.
D
The X starting coordinate of the tool. The tool will move
from this point to the XY starting point, in a 3-axis ramp
move. This is a "ramp-from" point.
E
The Y starting coordinate of the tool. The tool will move
from this point to the XY point, in a 3-axis ramp move.
This is a "ramp-from" point.
(Continued…)
All rights reserved. Subject to change without notice.
17-April-04
5-27
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Table 5-20, G169 Address Words (Continued)
Address
Words
Description
A
The distance the tool will step over (width of cut) as it mills
out the pocket. The step over selected may need to be
adjusted to ensure that excessive stock is not left on any of
the pocket sides.
B
The depth per pass. If a deep pocket is necessary, it might
not be feasible to take all the stock in one cut, so the Depth
of Cut can be programmed to allow two or more passes.
S
Finish stock. The CNC automatically executes a finish
pass after it roughs out the pocket. The finish stock
amount applies to sides and bottom. If you do not specify a
value, finish stock is not left.
I
The feedrate at which the tool will "ramp" into the pocket in
all three axes.
J
Rough-cycle feedrate.
K
Finish-cycle feedrate.
P
The Absolute Z position at the end of the cycle. Defaults to
H value.
Using Irregular Pocket in Subprograms
The Irregular Pocket is typically used with the main program. In cases
where the Irregular Pocket is being used in a subprogram, an M-code
must be used to specify the tool number whose tool diameter must be
used in the calculations of the Irregular Pocket. The M-code must be
placed immediately before the Irregular Pocket. If Irregular Pocket is
used in the main program, it is not necessary to use this M-code.
Format: MCode 9367 X (tool#)
Tool# is the number of the tool diameter whose diameter must be used in
the calculations of the Irregular Pocket.
Example:
M9367 X3
G169 W1 X2.0 Y2.0 (etc.)
This will use the diameter of Tool# 3 in the calculations of the Irregular
Pocket.
5-28
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Pockets with Islands (G162)
Format: G162 An Bn Cn Dn En
This cycle allows islands in irregular pockets. The main pocket must the
lowest subroutine number. Normally, this would be one (1). Pockets with
Islands can be programmed using:
•
•
•
DXF (see “Section 17, Using DXF for Pockets with Islands (G162)”)
CAM (see “Section 18, Example #12 Using CAM for Pockets with
Islands (G162)”)
Subroutines
More than one G162 Island cycle can be programmed at a time. They
may be strung together, but on separate lines. Islands can be
programmed inside of islands. Five islands can be put on a line. The
shape number subroutine number is used as inputs.. Refer to
Table 5-21.
Activate a tool prior to programming G78, so cutter diameter is known.
Table 5-21, G162 Address Words
Address
Word
A
B
C
D
E
Description
First island. Required.
Second island. Optional.
Third island. Optional.
Fourth island. Optional.
Fifth island. Optional.
Using Subroutines for Pockets with Islands
The program below is the same one used in the DXF portion with
subroutines added for the letters. In the third G162 some of the numbers
have negative sign (-) in front of them, this changes the side of the cutter
comp for the islands in islands. See Figure 5-13, Subroutines Pockets
with Islands Example Workpiece and Table 5-22, Pockets with Islands
Subroutines Programming Example.
All rights reserved. Subject to change without notice.
17-April-04
5-29
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Figure 5-13, Subroutines Pockets with Islands Example Workpiece
Table 5-22, Pockets with Islands Subroutines Programming Example
N1
N2
N3
N4
N5
N6
N7
N8
N9
N10
N11
N12
N13
N14
N15
N16
N17
5-30
G00 G17 G70 G90
T1D.0205 L-1 M6
S1250M3
M8
G53O01
G162 A2 B3 C4 D5 E6
G162 A7 B8 C9 D10
G162 A-11 B12 C-13 D-14
G169 W1 H0.1 Z-0.0050 C299. A0.0080 I5.0 J12.0 S0.0010
K10.0 P1
M2
O11
X1.1044 Y0.5
Z0.1
G01 Z-0.005
G01 X1.159 Y0.65
X1.2052
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
N18
N19
N20
N21
N22
N23
N24
N25
N26
N27
N28
N29
N30
N31
N32
N33
N34
N35
N36
N37
N38
N39
N40
N41
N42
N43
N44
N45
N46
N47
N48
N49
N50
N51
N52
N53
N54
N55
X1.2598 Y0.5
X1.2226
X1.2135 Y0.525
X1.1507
X1.1416 Y0.5
X1.1044
G00 Z0.1
M99
O12
X1.1634 Y0.56
Z0.1
G01 Z-0.005
G01 X1.1821 Y0.6112
X1.2007 Y0.56
X1.1634
G00 Z0.1
M99
O13
X1.4007 Y0.55
Z0.1
G01 Z-0.005
G01 X1.3612
G02 Y0.6 I-0.0312 J0.025
G01 X1.4007
G03 Y0.55 I-0.0707 J-0.025
G00 Z0.1
M99
O14
G0 X1.42Y.5
G1 X1.42Y.65
G1 X1.460 Y.65
G1 X1.460 Y.5
G1 X1.42 Y.5
M99
All rights reserved. Subject to change without notice.
17-April-04
5-31
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Irregular Pocket Examples
Example 1:
This example uses an irregular pocket cycle to cut the pocket shape.
Refer to Figure 5-14. Program the perimeter of the pocket in a
subprogram. The CNC calculates the moves to mill out the pocket.
Enter a 3/8" diameter tool in the Tool Page. This part program consists
of a main program and a subprogram. Refer to Table 5-23.
6.0
ABS
ZERO
2.5
.5 R
1.5
.75
1.5
1.0
1.0 R
2.5
G169
Figure 5-14, G169 Programming Example 1
Table 5-23, G169 Programming Example 1
1
2
3
4
5
6
7
8
9
10
11
12
13
14
15
5-32
G90 G70 G17
T1
G169 W1 H.1 Z-.125 D1.0 E-1.0 A.15 S.01 I7.5 J12.5
K9.5
G90 G00 T0 Z0
M2
O1
G90 G00 X0.0 Y0.0
G01 X2
G2 X2.5 Y-.5 R.5
G1 Y-1.5
X6
Y-3
G2 X5 Y-4 R1
G1 X1.25
G2 X.75 Y-3.5 R.5
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
16
17
18
19
G91 G1 Y1
G90 X0 Y-1.5
Y0
M99
Example 2:
Use an irregular pocket cycle to cut the pocket shape. Input the
"perimeter" of the pocket into a subprogram. The CNC will calculate the
moves to mill out the pocket. Input a 3/8" diameter tool in the Tool Page.
This part program consists of a main program and a subprogram. Refer
to Figure 5-15 and Table 5-24.
Rad. 1.25"
Rad. 0.75"
X0,Y0
X5,Y0
G169_2
Figure 5-15, G169 Programming Example 2
Table 5-24, G169 Programming Example 2
1
2
3
4
5
6
7
8
9
10
11
12
13
G90 G70 G0 T0 Z0
T1
G169 W99 H.1 Z-.25 C89.9 D0 E0 A.16 B.125 S.01
I7.5 J12.5 K9.5
G90 G00 T0 Z0
M2
O99
G90 G00 X-1.25 Y0
G2 X .125 Y 1.2437 R1.25
G1 X 5.075 Y .7462
G2 X5.075 Y-.7462 R.75
G1 X .125 Y -1.2437
G2 X -1.25 Y0.0 R1.25
M99
Figure 5-16, Example 2, Toolpath illustrates the toolpath used by the
CNC to mill out Example 2.
All rights reserved. Subject to change without notice.
17-April-04
5-33
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Figure 5-16, Example 2, Toolpath
Facing Cycle (G170)
Format: G170 Xn Yn An Bn Fn Hn Zn Dn En
Facing cycles simplify the programming required to face the surface of a
part.
Execution begins one tool radius from the D and E (start point). The
selected stepover determines the approach axes. Refer to Figure 5-17.
Figure 5-17, Face Cycle Tool Approach
Facing cycles can start in any corner of the surface and cut in any
direction, depending on the sign (+/-) of the X (Length) and A (Width)
values. Program a slightly oversized X and A to ensure complete facing
of the surface.
At the end of the cycle, the tool rapids to H, then rapids back to D and E
(start position).
5-34
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Table 5-25 describes the FACE POCKET entry fields.
Table 5-25, G170 Address Words
Address
Word
Description
Y
Y-axis length to be faced. Required.
X
X-axis length to be faced. Required.
A
Width of cut in the X-axis direction. When you do not enter
a value, the CNC defaults to 70% of the active tool radius.
Maximum step-over permitted is 70% of the active tool
radius.
Width of cut in the Y-axis direction. When you do not enter
a value, the CNC defaults to 70% of the active tool radius.
Maximum stepover permitted is 70% of the active tool
radius.
Feedrate used in cycle.
B
F
H
Z
D
E
The Absolute Z position before beginning the facing cycle.
This must be 0.1 inch (or 2 mm) above the surface.
Executed in rapid. Required.
Absolute depth of the finished surface. Required.
NOTE: Z must be lower than H. H is 0.1 inch (2.0 mm)
above the work surface.
X coordinate of the starting point. Defaults to current
position.
Y coordinate of the starting point. Defaults to current
position.
NOTE: Enter either an X or Y stepover only. Do not enter both.
NOTE: The Program Editor will allow you to inadvertently write a block
containing a stepover value greater than 70% of the active tool
radius. Test a program in the Draw Graphics Mode to reveal
this type of error.
NOTE: Z must be lower than H. H is 0.1 inch (2.0 mm) above the work
surface.
All rights reserved. Subject to change without notice.
17-April-04
5-35
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Circular Profile Cycle (G171)
Format: G171 Xn Yn Hn Dn Zn An Rn Bn Sn In Jn Kn Pn
The Circular Profile Cycle cleans up the inside or outside profile of an
existing circle.
When executed, the CNC rapids to Ramp#1 starting position, rapids to
H (StartHgt), then feeds to the depth of the first cut.
The machine feeds into the profile along Ramp #1, cuts the circle to the
specified D (Diameter) then ramps away from the work along Ramp #2.
When cutting an outside profile, the tool ramps into the work along Ramp
#1 and away from the work along Ramp #2 as illustrated in
Figure 5-18.
Di amet er
Di amet er
2
1
X, Y
X, Y
1
2
Ramp
Ramp
Inside
Outside
Figure 5-18, Ramp Position for Inside and Outside Profile
The Circular Profile Cycle automatically compensates for tool diameter.
Activate the correct tool diameter before the G171 block.
Table 5-26 describes the CIRCULAR PROFILE entry fields.
Table 5-26, G171 Address Words
Address
Word
X
Y
H
D
5-36
Description
X coordinate of the center. Default: present position.
Optional.
Y coordinate of the center. Default: present position.
Optional.
Z absolute starting (rapid) height (must be 0.1 inch or 2 mm
above surface to be cut into). Executed in rapid. Required.
Finished diameter of circle. If you enter a negative value,
both the direction of cut and the starting and endpoints
reverse. Required.
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Table 5-26, G171 Address Words (Continued)
Address
Word
Description
Z
Absolute depth of the finished profile. Required.
A
R
Setting for cutting on the inside of the profile (In) or the
outside (Out). Selection required. 0=In, 1=Out.
Ramp distance used for each pass. Optional.
B
Z-axis increment used for each pass. Optional.
S
I
Amount of stock left by the machine before the finish pass.
Default: 0. Enter a negative value to leave the stock
without making a finish pass. Optional.
Z-axis feedrate. Optional.
J
Rough-pass feedrate. Optional.
K
Finish-pass feedrate. Optional.
P
Retract Hght.
If you enter a Depth Cut = B (Z Max.cut), the CNC executes the number
of passes required to get from the H (Z Start Hgt.) to Z (Z Depth),
cutting to the Depth Cut = B (Z Max.cut) on each pass.
When you enter an S (Finish Stock) value, the CNC leaves the
specified stock on the profile and depth for a finish pass. The CNC
finishes to the entered diameter on the finish pass. Enter a negative S
(Finish Stock) to leave the finish stock without making a finish pass.
If you do not enter a J (Rough Feed) or K (Finish Feed) value, the CNC
executes feed moves at the current feedrate. J controls feedrate of the
roughing cycle. K controls the feedrate of the finishing cycle.
All rights reserved. Subject to change without notice.
17-April-04
5-37
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Rectangular Profile Cycle (G172)
Format: G172 Xn Yn Hn Mn Wn Zn An Rn Un Bn Sn In Jn Kn Pn
The Rectangular Profile Cycle cleans up the inside or outside profile of a
rectangle. When run, the CNC rapids to the Ramp #1 starting position,
rapids to H (Z StartHgt), and then feeds to the depth of the first cut.
The machine feeds into the profile along Ramp #1, cuts the rectangle to
the M (Length) and W (Width) specified then ramps away from the work
along Ramp #2.
When cutting an inside profile, the Graphic Menu displays ramp moves.
When cutting an outside profile, the tool ramps into the profile along
Ramp #1 and away from the profile along Ramp #2, as illustrated in
Figure 5-19.
L en gt h
Len g t h
2
1
X, Y
Wi d t h
Rad i u s
Wi d t h
Radi u s
1
Inside
X, Y
Ramp
2
Ramp
Outside
Figure 5-19, Inside and Outside Profile Ramp Moves
The Rectangular Profile Cycle automatically compensates for tool
diameter. Activate the correct tool diameter before the G172 block.
Table 5-27 describes the Outside Profile Ramp Moves entry fields.
Table 5-27, G172 Address Words
Address
Word
X
Y
H
M
W
Z
Description
X coordinate of the center. If no coordinate is entered, the
CNC centers the pocket at its present position.
Y coordinate of the center. If no coordinate is entered, the
CNC centers the pocket at its present position.
The Absolute Z position before beginning to mill the pocket.
This must be 0.1 inch (or 2 mm) above the surface.
Finished length of rectangle. Required.
Finished width of rectangle. Required.
Absolute depth of the finished profile. Value required.
(Continued…)
5-38
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Table 5-27, G172 Address Words (Continued)
Address
Word
Description
A
0 = Inside
1 = Outside
R
U
Radius of the ramping moves. Required.
Corner radius setting. If the programmer enters a negative
value, both direction of cut and the starting and endpoints
reverse. Optional.
Maximum Z-axis increment used for each pass. Optional.
Amount of stock left by the machine before the finish pass.
Default: 0. If the programmer enters a negative value, the
CNC will leave the stock without making a finish pass.
Optional.
Z-axis feedrate. Optional.
Rough-pass feedrate. Optional.
Finish-pass feedrate. Optional.
Retract Hgt.
B
S
I
J
K
P
When you enter a value, the CNC executes the number of passes
required to get from the H (Z Start HGT) to the Z (Z Depth), cutting the B
(Z Max.cut) on each pass.
When you enter an S (Finish Stock) value, the CNC leaves the specified
stock on the profile and depth for a finish pass. The CNC cuts the
rectangle to the M (Length), W (Width), and Z (Z Depth) dimensions on
the finish pass. Enter a negative S (Finish Stock) to leave the finish stock
without making a finish pass.
When you do not enter a J (Rough Feed) or K (Finish Feed), the CNC
executes feed moves at the current feedrate. J (RoughFeed) controls the
feedrate of the roughing cycle. K (Finish Feed) controls the feedrate of
the finishing cycle.
All rights reserved. Subject to change without notice.
17-April-04
5-39
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Thread Mill Cycle (G181)
Format: G181 Xn Yn Hn Zn Dn An Rn Bn Cn Sn In Jn Kn En Vn
Use the thread milling for cutting inside or outside threads. It will cut
either Inch or MM, left or right hand, and Z movement up or down. A
single tooth or multi-toothed tool may be used. Start can be at the top or
bottom of the hole or boss. The tools are set, as you would normally set
TLO.
Programming the Thread Mill Cycle
To program the Thread Mill Cycle:
1. In Edit mode, press Thread Mill (F9) and to display the G181
Thread Mill pop-up menu (refer to Figure 5-20).
2. Complete the entry fields (refer to Table 5-28, G181 Address Words),
and press ENTER.
When cutting a thread, the tool ramps into the cut as illustrated in
Figure 5-20.
Figure 5-20,Thread Mill Pop-up Menu
Table 5-28, G181 Address Words describes the Thread Mill Cycle entry
fields.
5-40
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Table 5-28, G181 Address Words
Address
Word
Description
X
X coordinate of the center of hole or boss X-axis, if not
stated must be position at center before calling cycle. Will
return to this point when cycle is done. (Optional)
Y
Y coordinate of the center of hole or boss X-axis, if not
stated must be position at center before calling cycle. Will
return to this point when cycle is done. (Optional)
H
The Absolute Z position before beginning to mill the pocket.
Start height Distance above to rapid to before feeding to
cut depth. This must be 0.1 inch (or 2 mm) above the
surface. (Required)
Z
Start depth at which threading tool is going to start cutting.
Care should be taken if Z movement is down and in a blind
hole that there is clearance at the bottom of hole or boss so
the tool does not smash and break. (Required)
D
Diameter of hole or boss. Internal will be root diameter of
thread, external will be major diameter of thread.
(Required)
A
0 = inside of hole, 1= Outside of boss. (Required)
R
Ramp distance cycle will arc into cut and arc off of cut; this
is the size of the radius when arcing on or off. (Required)
B
Threads per inch (T.P.I.) or Lead of thread. (Required)
C
Number of turns around the hole or boss cutter will make.
Using plus (+) or minus (-) controls direction of Z-axis
movement. (Required)
S
Depth of cut per pass, this plus the number of pass (E) and
start diameter will give the depth of thread. (Required)
I
Number of loop in a cycle and direction + CCW and –CW
this number. Will be the same as (C). (Required)
J
Rough federate. (Optional)
K
Finish federate. (Optional)
E
Sets number of pass it will take to get to depth. (Required)
V
Taper in degrees. For straight thread, leave blank.
(Optional)
Tool height is set the same as any other tool.
A tool diameter also has to be set as cutter compensation is built into
Cycle.
All rights reserved. Subject to change without notice.
17-April-04
5-41
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
If X and Y are not programmed position tool at center of hole or boss:
•
Tool will come down to start height, move to start position X and Y.
•
Move down to start cut position (H).
•
Arc into first cut position.
•
Spiral up or down depending if (C) is plus or minus and go
counterclockwise or clockwise depending if (I) is plus or minus.
•
Arc of Ramp distance.
•
Move back to (H) height.
•
Move to X and Y start position; move in depth of cut (S).
•
Repeats process until to depth.
•
It will repeat last cut.
When cutting taper, care must be taken with (R) ramp move. (R) ramp
distance this must greater than depth of thread.
Sample Thread Milling Cycle Program
1
2
3
4
5
6
7
8
G90 G70 G0 G17 G0
T1 M6
S1000 M3
X0 Y0
G181 H0.1 D2. Z-1. A0 R0.25 B10. C11 S0.02 I11 J10.0 K10.0 E2
Z5
M5
M2
This program threads at X0 Y0, starting height 0.1, starting diameter 2,
starting depth –1, inside of hole, ramp distance 0.25, 10 threads per inch,
11 turns around the hole, 0.02 depth of cut per pass, 11 loops in a cycle
(+ CCW) [the same as (C)], 10.0 rough federate, 10.0 finish federate, and
2 passes to get to depth.
5-42
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Plunge Circular Pocket Milling (G177)
Format: G177 Xn Yn Hn Zn Dn An Bn In Jn Sn Kn Pn
Use the plunge circular pocket cycle (G177) for carbide tooling, when a
multiple-axis ramp-in move is not possible. The Z-axis will plunge (singleaxis) to programmed depths. You must drill a start hole prior to using this
cycle. Activate the tool prior to G177 so that tool diameter is known. The
tool is not required to be at the center of the pocket, as the cycle has
variable words for X and Y center. If you do not program X and Y
variable words with G177, then the CNC will use the current position as
the pocket center. Refer to Table 5-29.
Table 5-29, G177 Address Words
Address
Word
Description
X
Center of the pocket in X-axis. Defaults to current position.
Y
Center of the pocket in Y-axis. Defaults to current position.
H
The Absolute Z position before beginning to mill the pocket. This
must be 0.1 inch (or 2 mm) above the surface. Executed in rapid.
Absolute depth of pocket.
Z
D
A
B
I
J
S
K
P
Diameter of pocket.
+D dimension = climb (CCW).
-D dimension = conventional (CW).
Maximum tool stepover (must be less than tool diameter). If +A
dimension = outward spiral.
-A dimension = inward spiral. On inward spirals, the tool moves
to O.D. at 0 degrees, and begins the roughing process there (3
o'clock). Defaults to tool radius.
Maximum Z depth per pass (For example, if Z = -1, and
B = 0.5, the pocket will be roughed out in two levels.) B is
positive. Defaults to tool diameter (depth), less finish stock.
Z feedrate for plunge move. The tool will feed to the first depth of
cut with a plunge move. Defaults to last programmed feedrate.
Feedrate of rough cycle used to mill out the pocket. Defaults to
last programmed feedrate.
Finish stock amount per side (including bottom). Positive = leave
stock and execute finish pass. Negative = leave stock without
executing a finish pass. If no value is given, no finish stock is left.
Finish-pass feedrate. Defaults to last programmed feedrate.
Z-axis absolute-retract height (must be equal to or above H).
Executed in rapid. Defaults to H value.
All rights reserved. Subject to change without notice.
17-April-04
5-43
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
The required position of the start hole is as follows:
1. For inward to outward cutting (+A): at the hole center.
2. For outward to inward cutting (-A): start hole must be at the 3 o'clock
position on the pocket perimeter, less finish stock, less tool radius.
3. Drilled to a sufficient depth.
4. The axes must be positioned over the start hole prior to programming
this cycle.
5. If you position the tool at the pocket center and omit XY words from
G177 block, the CNC will use current position as pocket center.
Plunge Rectangular Pocket Milling (G178)
Format: G178 Xn Yn Hn Zn Un An Bn In Jn Sn Kn Pn
Use the plunge rectangular pocket cycle (G178) for carbide tooling,
where a multiple-axis ramp-in move is not possible. The Z-axis will
plunge (single-axis) to the programmed depth. You must drill a start hole
previous to the G178 cycle. Activate a tool prior to programming G178,
so cutter diameter will be known. Position the tool at the center of the
pocket prior to G178, or use the X and Y words. Refer to Table 5-30.
Table 5-30, G178 Address Word
Address
Word
X
Y
M
W
H
Z
U
A
B
I
5-44
Description
X center of pocket. Optional.
Y center of pocket. Optional.
Length of pocket in X-axis. Required.
Width of pocket in Y-axis. Required.
Z absolute starting (rapid) height (0.1 inch or 2 mm above
surface). Required. Executed in rapid.
Absolute depth of pocket. Required.
Actual corner radius of pocket (all four corners). Must be
equal or greater than tool radius. Defaults to tool radius.
Maximum tool stepover (must be 70% or less of tool
diameter). Positive = CCW. Negative = CW. Defaults to
half tool diameter.
Maximum Z depth per pass. (For example, if you program
Z to be -1, and B to be .5, the CNC will rough out the
pocket in two levels.) B is positive. Defaults to tool
diameter (depth), less finish stock.
Z Plunge feed. The tool will plunge to the first depth of cut
with a single-axis Z move from the centerline of the lowerleft radius. Defaults to last programmed feedrate.
(Continued…)
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Table 5-30, G178 Address Word (Continued)
Address
Word
J
S
K
P
Description
After the plunge move, the tool will rough mill the pocket, at
feedrate J. Defaults to last programmed feedrate.
Finish stock amount per side (including bottom).
Negative = stock will be left, but no finish pass will occur.
Positive = leave stock and execute finish pass. If not
programmed, no finish stock is left.
Finish-pass feedrate. Defaults to last programmed
feedrate.
Z-axis absolute finish height (must be equal to or above H).
Defaults to H value. Executed in rapid.
WARNING: When you cut a pocket inside another
pocket, you must set P above the highest
pocket. At the end of each pocket, the tool
will rapid to P, then rapid to the start
position.
You must position the start hole at the center of the pocket prior to G177
and drill to a sufficient depth.
Mold Rotation (G45)
NOTE: Activate the required plane (G17, G18 or G19) prior to G45.
I, J centerline of rotation values are used only if the other axis is not 0.
For X rotation, I = Y and J = Z.
For Y rotation, I = X and J = Z.
For Z rotation, I = X and J = Y.
A Mold Rotation (G45) is used to mill cylindrically symmetrical cavities
and cores. A cylindrically symmetrical shape is a shape defined by
rotating a profile around an axis. Refer to Table 5-31, G45 Address
Words and Figure 5-21, XY-Axis Mold Rotation.
There are two categories of mold rotation:
q
Rotation around X- or Y-axes
q
Rotations around the Z-axis
Format: G45 An Bn Cn Fn Rn X (or Y) (or Z) In Jn Kn
All rights reserved. Subject to change without notice.
17-April-04
5-45
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Table 5-31, G45 Address Words
Address
Word
A
B
C
F
R
X (or Y)
(or Z)
I
J
K
Description
Absolute start angle. Starting angle of the rotation.
Required.
Absolute end angle. Final angle of the rotation. Required.
Number of subprogram cycles executed between start and
stop angles. One cycle equals one forward plus one
reverse subprogram pass. Set low for rough cycle. Set
high for finish cycle. Required.
Forward subprogram call. Required.
Reverse subprogram call. Required.
Axis of rotation select. Required.
The centerline of rotation in the “other” axis. Other axis is
X or Y (not the rotation axis described in XY).
Second position coordinate of the rotated axis in Z. Use
only for Z rotation. Optional.
Z-axis rotation of XY-axis mold. Calculate CCW from XY
plane 3 o'clock. Use only for X or Y rotation. Optional.
Figure 5-21, XY-Axis Mold Rotation
5-46
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Rotations Around X and Y Axes (Small Radius)
Each Mold Rotation block requires two subprograms: a forward
subprogram to define the profile moving away from the starting point and
a reverse subprogram to define the profile moving back to the starting
point. Refer to Figure 5-22.
Forward Subprogram
(First Half Of Cycle)
+Z
Axis Of
Rotation
Cycle
Starting Point
Incremental Move
Direction
-Y
Subprogram
End Point
Reverse Subprogram
(Second Half Of Cycle)
+X
+Z
Axis Of
Rotation
Subprogram
End Point
Incremental Move
Direction
-Y
Subprogram
Starting Point
+X
Figure 5-22, Subprogram Orientation
All rights reserved. Subject to change without notice.
17-April-04
5-47
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
In one cycle, the CNC executes the forward subprogram to the profile
endpoint, then executes the reverse subprogram back to the starting
point. Each cycle is incremented around the axis of rotation from the
start angle (A) to the end angle (B). The amount of rotation in each
increment is determined from the number of cycle’s (C) and the size of
the start and end angle values programmed into the block.
The cycle starts cutting the first subprogram (profile) from the machine’s
present position. Refer to Figure 5-23.
Direction Of Incremental Moves In
Forward Subprogram (A to B)
Direction Of Incremental Moves In
Reverse Subprogram (B to A)
+Y
Starting and Endpoints
for Ramp Moves
+X
Point A
Centerline
Tool Comp Ramp On & Off Moves
(Permits Correct Activation Of
Alternating RH & LH Tool Comp)
Point B
MOLDSUB1
Figure 5-23, Subprogram Specifics
In small radius rotations, subprogram start and endpoints can lie along
the centerline of rotation. All subprogram moves must be incremental.
Both subprograms must produce profiles that are exactly the same
shape, but that execute in opposite directions.
When the rotation is around the X-axis, all of the moves in the
subprogram must be contained in the +Y half of the XY plane. When the
rotation is around the Y-axis, all of the moves in the subprogram must be
contained in the +X half of the XY plane.
If tool compensation is not used, the path in the subprogram must be
adjusted for the radius of the tool. If cutting a core, the path must be
increased by one tool radius. If cutting a cavity, the path must be
reduced by one tool radius.
5-48
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
To use tool compensation, write compensated moves in the
subprograms. Tool compensation for each subprogram must be on
opposite sides.
Each time you activate tool compensation, you must program a ramp
on/off move for position adjustment. Add ramp moves to subprograms as
shown.
Refer to ”Programming Concepts” in “Section 1” for information on using
tool length offset and diameter compensation with ball-end mills.
The rotation occurs around the axis selected in the axis of rotation
(centerline of rotation). Use I and J values to define the position of the
centerline when it is not located at the axis zero (X0, Y0, Z0). Refer to
Figure 5-24.
Figure 5-24, Axes of Rotation
All rights reserved. Subject to change without notice.
17-April-04
5-49
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
When the rotation is around the X-axis, the centerline is defined by the Yaxis position (in the I field) and the Z-axis position (in the J field).
When the rotation is around the Y-axis, the centerline is defined by the Xaxis position (in the I field) and the Z-axis position (in the J field).
The start angle (A) and the end angle (B) are absolute start and stop
angles of the rotation. Use negative angle values to cut cavities and
positive angle values to cut cores.
To execute a Mold Rotation that requires more than one pass, write the
subprograms for the finished shape and call the subprograms from more
than one Mold Rotation block.
Adjust the starting position and J value of each block so that each pass
comes closer to the finished shape. Reverse the sequence shown in the
figure to cut a core. Refer to Figure 5-25.
Figure 5-25, Cutting a Cavity Using More Than One Pass
X- and Y-axis rotations can be rotated around the Z-axis by entering a Z
angle (K). Refer to Figure 5-26.
Figure 5-26, Rotating XY Mold Rotations Around Z
5-50
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Rotations Around X and Y Axes (Large Radius)
The mold rotation cycle starts executing the subprograms at the
machine’s present position.
To cut a large radius rotation, start the cycle at the required distance from
the centerline. The additional distance is automatically added to the
radius of the rotation.
If the rotation does not swing a full 180°, the starting position will be a
point on the starting angle the required distance from the centerline.
Refer to Figure 5-27.
Z
96 Inch R
+X
Z
Centerline
Subprogram Profile
X0, Y0, Z0
+Y
o
-70
96 Inch Radius
o
40
+X
Starting Position
-70 o , 96 inch from center
(X0, Y32.833, Z-90.21)
LG-RAD2
Figure 5-27, Large Radius Mold Rotation
All rights reserved. Subject to change without notice.
17-April-04
5-51
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Rotation Around the Z-Axis
The centerline of rotation is parallel to the Z-axis (Axis Rotation). The I
and J values are the X and Y coordinates of the centerline. Enter the X
coordinate in the I field and the Y coordinate in the J field. Refer to
Figure 5-28.
+Z
-X
Centerline of Rotation
+Y
-Y
+X
-Z
MOLDZ
Figure 5-28, Z-Axis Mold Rotation
The machine must be positioned at the center of the rotation when the
cycle starts. The finished shape will be centered on the starting position.
The Z-axis position of the starting point determines the Z-axis position of
the finished shape.
5-52
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
All of the moves in subprograms for Z-axis rotations must be contained in
the +X half of the XZ plane. Rules for using tool compensation are the
same as for Y- and X-axis rotations. Refer to Figure 5-29.
Direction Of Incremental Moves In
Forward Subprogram (A to B)
Direction Of Incremental Moves In
Reverse Subprogram (B to A)
Tool Comp Ramp On And Off Moves
(Permits Correct Activation Of
Alternating RH & LH Tool Comp)
+Z
Starting and Endpoints
for Compensation Ramp
Moves
Point B
Point A
+X
XZ Plane View
Figure 5-29, Z-Axis Rotation Subprogram Details
Z-axis rotation start and end angles are shown. Refer to Figure 5-30.
+Z
+Y
EndAngle
-X
-Y
StartAngle
+X
-Z
Figure 5-30, Z-Axis Rotation Start and End Angles
All rights reserved. Subject to change without notice.
17-April-04
5-53
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Example 1:
The following programming example mills out a handle-mold core using
G45 around the Y-axis. Refer to Figure 5-31 and Table 5-32.
Figure 5-31, Handle Mold Core
Table 5-32, G45 Programming Example 1
Main Program
O2020 * HANDLE.G
G90 G70 G0 G17
X1.625 Y1.5
G90 G1 Z0 F12
G45 A0 B180 C10 F15 R16 Y I1.625 J0
G90 G0 Z1.0
M2
Forward Subprogram (O15) Reverse Subprogram (O16)
O15 * HANDLE-FWD
O16 * HANDLE-REV
G91 G1 X-.25
G91 G3 X-.25 Y-.0625 R3
G2 X-.25 Y.27 R.25
G3 X-.25 Y-.25 R.25
G2 X.125 Y3 R12
G2 X.125 Y-2 R9
G3 X-.125 Y2 R9
G3 X-.125 Y-3 R12
G2 X.25 Y.25 R.25
G3 X.25 Y-.27 R.25
G2 X.25 Y.0625 R3
G1 X.25
M99
M99
5-54
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Example 2:
The following example mills a dish shape. The forward and reverse tool
paths are programmed in the XZ plane, with tool compensation. Refer to
Table 5-33.
Table 5-33, G45 Programming Example 2
Main Program
O99 * MOLD-Z
G90 G70 G0 T0 Z0
X0 Y0
T1 * .25 BALL-MILL
Z.225
G1 Z0 F3
G45 A0 B350 C18 F1 R2 Z I0 J0
G17 G90 G0 T0 Z0
M2
Forward Subprogram
O1 * FWD SUB
G18 G91 G42 Z-.25 F3
X.5
G2 X2 Z.125 R5 F8
G1 X.125
G40 Z.25
M99
Reverse Subprogram
O2 * REV SUB
G41 Z-.25
X-.125
G3 X-2 Z-.125 R5
G1 X-.5
G40 G1 Z.25
M99
NOTE: The tool diameter in the Tool Page could be set to .270 for
roughing (at C18 - 18 cycles). Then for finishing, set tool
diameter to .2500, and increase B to 359, and C to 180.
All rights reserved. Subject to change without notice.
17-April-04
5-55
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Elbow Milling Cycle (G49)
Format: G49 Bn Kn An Cn In Jn Dn Fn En Rn Zn Hn Un Sn Vn
Elbow Milling cycles simplify the required programming for milling elbow
shaped cavities and cores. Finished elbows can have the same radius at
each end (bent cylindrical shape), or a different radius at each end (bent
conical shape). Refer to Table 5-34.
NOTE: Position the tool at the start position prior to G49.
Table 5-34, G49 Address Words
Address
Word
B
K
A
C
I
J
D
F
U
V
S
Description
Start radius. Required.
End radius. Required.
Included angle of elbow.
Default: CCW (Counterclockwise)
To change direction, use the D parameter.
NOTE: Must specify A or F, but not both.
Number of cycles to complete elbow. (Positive for female
cavity and negative for male core.) Required.
Absolute elbow origin in X.
Absolute elbow origin in Y.
Direction of cone from starting point:
+1 CCW (Counterclockwise)
–1 CW (Clockwise)
If you use D, you must use it with A or F, but not both.
End angle from 3 o’clock using center (I,J) as polar
reference. Must be used with D if used.
NOTE: Must specify A or F, but not both.
Rough-cycle feedrate.
Finish-cycle feedrate.
Finish-stock amount.
NOTE: Next four variables must be used as a group. They provide XY
and Z positions to the start of the conic cut.
E
Start angle, referenced from polar center (I,J).
R
Radius to the centerline of the cone, referenced from polar
center (I,J).
Z
Absolute rapid height.
H
Start height in Z.
5-56
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
The Elbow Milling Cycle starts at the machine’s present position. The
CNC executes passes back and forth around the elbow inner radius from
the start radius to the end radius. The tool is incremented further into the
cavity (or around the core) at the end of each pass until the elbow is
complete. The cycle stops at the opposite side of the elbow at the same
Z-axis position from which it started. Refer to Figure 5-32.
Figure 5-32, Elbow Cavity and Core
You cannot use tool compensation with the Elbow Milling Cycle. When
cutting a particularly deep elbow, it may be necessary to cut the shape in
several passes. The easiest way to do this is to program the elbow in a
subprogram. The main program should consist of moves to position the
machine at consecutively lower Z-axis starting positions. The
subprogram is called at each successive starting position. Refer to
Figure 5-33.
+Z
+Y
Starting Position
+X
CW Execution Of Moves For Elbow Cavity
Figure 5-33, Execution of Elbow Milling Cycle Moves
All rights reserved. Subject to change without notice.
17-April-04
5-57
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Carefully consider the starting position of the Elbow Milling Cycle. The
distance between the starting point and the XY center determines the
elbow’s inner radius. The line between the starting point and the XY
center is the zero degree reference for the included angle. If you leave
the X and Y center values blank the CNC uses X0, Y0. Refer to
Figure 5-34.
InclAngle
(Ccw, Incremental)
EndRad
+Y
+Z
90°
XCenter
YCenter
0°
Major
Radius
Starting Point
(Present Location)
StartRad
+X
Figure 5-34, Elbow Milling Cycle Details
When the line between the starting point and the X Center, Y Center
does not lie along an X or Y-axis, the orientation of the finished elbow will
shift around the XY center accordingly. Refer to Figure 5-35.
+Y
+Y
90°
90°
90°
XCenter
YCenter
+Y
+X
+X
Starting
Point
Starting
Point
XCenter
YCenter
+X
Starting
Point
XCenter
YCenter
Figure 5-35, Starting Points Effect On Orientation
5-58
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
The distance between the starting point and the XY center determines
the elbow inner radius. Moving the starting point away from the XY
center increases the overall size of the finished elbow as shown. Refer to
Figure 5-36.
+Y
+Y
+X
+X
Starting Point
XCenter
YCenter
Starting Point
XCenter
YCenter
Figure 5-36, Starting Points Effect On Size
The Cycles (C) value determines the number of passes used to cut the
elbow. A negative cycle value cuts a core while a positive cycle value
cuts a cavity. Refer to Figure 5-37.
+Z
XY Plane
Negative Cycles (core)
(Elbow Cuts Above XY Plane)
Cycle Starting Point
-Z
Positive Cycles (cavity)
(Elbow Cuts Below XY Plane)
ELBSIDE
Figure 5-37, Core and Cavity Detail
All rights reserved. Subject to change without notice.
17-April-04
5-59
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Programming an Elbow Milling Cycle with unequal start radius and end
radius values produces a conical elbow. Refer to Figure 5-38.
+Z
+Y
EndRad
XY Center
StartRad
+X
EndRad Greater Than StartRad
Figure 5-38, Conical Elbow Details
Example:
The programming example in Table 5-35 machines an elbow cavity.
Table 5-35, G49 Programming Example
N1
N2
N3
N4
N5
N6
N7
N8
N9
N10
N11
N12
N13
5-60
O49 * ELBOW.G
G90 G70 G0 G17
T0 Z0
X0 Y0
T1 * .25-BALL
X3.125 Y1.125
Z.225
G1 Z0 F10
G49 B.875 K.875 A90 C8 I1.125 J1.125
G90 G0 Z.225
T0 Z0
X0 Y0
M2
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Subprograms
Program repetitive sequences or patterns in a subprogram. Enter
subprograms in the program after the end of the main program. Call
subprograms from the main program. Refer to Table 5-36.
Table 5-36, Subprogram Addresses
M98 Pn
M99
Oxxxx
Pn
Jump to subprogram.
Return to main program.
Subprogram label. Up to 4 digits.
Subprogram number to jump to.
A subprogram can use any code or move type. For example, to cut a
contour twice (one rough pass and one finish pass), program it as a
subprogram. You can call the subprogram from the main program as
many times as required, but you enter the parameters only once.
Subprogram(s) must be stored in the same file as the main program that
calls them.
Subprogram Addresses
Examples:
M98 P2000 commands a jump to subprogram O2000.
Following the program number, blocks in a subprogram are numbered as
in normal programming, as in the following example:
N2000 O2000 * SUBPROGRAM #2000
N2001 * blocks in program
N2002
N2003 etc.
You can store subprograms anywhere in the program after the main
program. They do not have to be entered in numerical order or begin on
any specific block number. Refer to Table 5-37.
Table 5-37, Subprogram Called from a Main Program
Main Program
N1 O3 *SUB-EX1
N2
N3 M98 P100
N4
N5
N6
N7
N8 M02
All rights reserved. Subject to change without notice.
17-April-04
Jump to N67 to execute subprogram 100.
5-61
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Table 5-37, Subprogram Called from a Main Program (Continued)
Subprogram
N67 O100
CNC jumps to here at N3, completes subprogram
until it reaches M99 (N71), and then returns to the
main program at N4.
N68
N69
N70
N71 M99
Repetition of Subprogram (Loop)
Format: M98 Pxxx Lxx
L is the number of repetitions of the subprogram.
Example:
M98 P2000 L12
The block commands twelve repetitions of subprogram number 2000.
The maximum number of repetitions is 9999.
Calling a Subprogram from a Subprogram
Calling a subprogram from another subprogram is referred to as nesting.
The maximum number of programs that can be nested is ten.
The method of calling an additional subprogram is similar to calling the
first. Refer to Table 5-38.
Table 5-38, Nesting Subprograms
Main Program
N1 O9 *SUB-EX2
N2
N3
N4 M98 P101
N5
N6
N7
N8 M02
Flow of Program
During Call of Additional Subprogram
Jump to 1st subprogram N501 from main
program at N4.
st
Return from 1 subprogram.
Return to N1 after all subprograms are complete.
1st Subprogram
N501 O101
N502
(Continued…)
5-62
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Table 5-38, Nesting Subprograms (Continued)
Main Program
N503
N504
N505 M98 P200
N506
Flow of Program
During Call of Additional Subprogram
Jump from 1st subprogram to 2nd subprogram
occurs at N505. Executes N600 to M606 (M99).
Return to N506 after 2nd subprogram is
completed (M99). Finish 1st subprogram.
N507
N508
N509 M99
Return to main program at N5.
2nd Subprogram
N600 O200
N601
N602
N603
N604
N605
N606 M99
Jump to N506.
Example:
Mill out a series of identical slots in a plate. Each slot is 1/2" wide and
.3750" deep. Slot 1 is programmed in a subprogram. All XY dimensions
will be incremental to enable you to position the slot anywhere on the
coordinate system. Refer to Figure 5-39.
1.0 (25.4)
3.5 (88.9)
1.0
(25.4)
Figure 5-39, Subprogram Programming Example
All rights reserved. Subject to change without notice.
17-April-04
5-63
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
The main program will position the cutter for each slot and call the
subprogram that mills out the slots. Subprogram O100 uses incremental
values to enable you to position the slot at various positions on the work.
For all three slots, you must position the cutter before you call the
subprogram. Refer to Table 5-39.
Table 5-39, Subprogram Programming Example
Blk #
N1
N2
N3
N4
N5
N6
N7
N8
N9
N10
N11
N12
5-64
Block
O12 *SLOTS-MAIN PROGRAM
G90 G70 (G71) G0 G17 T0 Z0
X-2 (X-50) Y2 (Y50)
T1 * 1/2" MILL
X1 (X25.4) Y-1 (Y-25.4) Z.1
(Z2.54) M98 P100
Y-2 (Y-50.8) M98 P100
Y-3 (Y-76.2) M98 P100
T0 Z0
X-2 (X50.8) Y2 (Y50.8)
M02
Description
Define program #12, program name.
Set absolute inch, rapid, XY plane,
cancel tool, Z0.
Move to X-2 Y2.
Activate Tool #1.
Move to slot location #1 and call sub.
Move to slot 2 and calls sub.
Move to slot 3 and calls sub.
Cancel tool offset and raises Z.
Move to X-2 Y2.
End program, reset to N1.
O100 *SLOTS-SUBPROGRAM
Define this as program #100, and
gives name.
N13
G90 G1 Z-.375 (Z-9.53) F3.5
(F89)
Feed Z to -.3750" in absolute.
N14
N15
N16
G91 X3.5 (X88.9) F10 (F254)
G90 G0 Z.1 (Z2)
G91 X-3.5 (X-88.9)
N17
G90 M99
Feed X 3.5" incrementally.
Rapid Z to 0.1" absolute.
Rapid X-3.5000", return to start
point.
Set Absolute Mode, end sub, return
to main.
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
End of Subprogram (M99) with a P-Code
M99 Pxxx
When the End of Subprogram (M99) command contains a P-code, the Pcode refers to the block number in the main program to which the
subprogram returns.
Example:
M99 P70
At N30, the CNC will execute the subprogram and then return to N70
(skipping N40 to N70) in the main program. From N70 it will resume
main program execution.
The subprogram will return the program to N70 of the main program,
skipping N40 through N60. Refer to Table 5-40.
Table 5-40, M99 P-Code Usage
Main Program
N10
N20
N30 M98 P100
N40
N50
N60
N70
N80
N90 M2
Subprogram
N110 O100
N120
N130
N140 M99 P70
Call subprogram.
After complete subprogram, return to N70 in
main.
Subprogram for Multiple Parts Programming
To set up a subprogram to machine multiple parts, follow this method.
In this example, a table has two vises installed. Each table holds a part
of identical configuration. The same tool does all the work.
1. Program the machining sequence as a subprogram in Absolute or
Incremental Mode.
2. When the sequence is finished on Part #1, program a coordinate shift
(G92 or G53) and recall the subprogram.
3. If you program the subprogram incrementally, you do not have to shift
the zero point. If programmed in absolute, then use a coordinate
(zero) shift.
All rights reserved. Subject to change without notice.
17-April-04
5-65
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Loop and Repeat Function
In some cases, it is simpler to command a program block or series of
blocks to loop (repeat), rather than to program the block(s) several times.
Format:
N680 LOOP nnnn
N685 .
.
.
N695 END
LOOP instructs the CNC to execute the blocks following block N680 until
END. The block is repeated nnnn times. Subprogram calls, axes moves,
M-codes, etc. are all available within a "loop".
Each LOOP must have an END. Nesting loops (one loop inside of
another) is possible, to 10 levels deep.
The full body of the LOOP command (LOOP to END) must be contained
in the main program or the subprogram in which it was initiated.
Example:
In the following program example, M and S codes are omitted. The
program assumes that a manual tool change machine is used (no ATC).
Check your machine tool manual for details on programming M, S, and T
codes. Refer to Figure 5-40 and Table 5-41, Loop Programming
Example.
Tooling to be used:
Tool 1 = #4 centerdrill
Tool 2 = 1/4" diameter twist drill
Tool 3 = 3/8" diameter end mill
2.0"
(50.8mm)
.75" (19.05mm) Typ.
X0Y0
2.5"
(63.5mm)
8.0"
(203.2mm)
.50" (12.7mm)
.25" (6.35mm)
Dia.
6 pos.
5.0"
(127mm)
7.5"
(190.5mm)
3.0"
(76.2mm)
SUBPR_EX2
R=5.0"
(127mm)
90 deg.
Figure 5-40, Loop Programming Example
5-66
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Table 5-41, Loop Programming Example
Blk. #
N1
N2
N3
N4
Block
O100 * EXAMPLE
G90 G70 (G71) G0 T0 Z0
N11
X-2 (X-50) Y2 (Y50)
T1 * #4 CTR-DRL (6.35
CRT-DRL)
G81 Z-.23 (Z-.5.84) R.1 (R2)
F8 (F203)
M98 P1
T2 * 1/4" DRL (* 6.35 DRILL)
G83 Z-.45 (Z-11.43) R.1 (R2)
F10 (F254) I.15 (I3.81)
M98 P1
T3 * 3/8" MILL (* 9.525
MILL)
G41 X-.3 (X-76.2) Y0
N12
N13
N14
N15
Z.1 (Z2)
G1 Z-.38 (Z-9.65) F13 (F330)
X8 (X203.2)
X7.5 (X190.5) Y-2.5 (Y-63.5)
N16
N17
G3 X7 (X177.8) Y-3 (Y-76.2)
I0 J-.5 (J-12.7)
G1 X5 (X127)
N18
X0 Y-2.5 (Y-63.5)
N19
N20
N21
N22
Y.3 (Y8)
G0 Z.1 (Z2)
G40 X-.3 (X-8)
T0 Z0
N23
N24
N25
N26
N27
X-2 (X-50) Y2 (Y50)
M2
N5
N6
N7
N8
N9
N10
O1 * HOLE LOCATIONS
SUB.
Description
Program name and number.
Set modes. Cancel tool. Rapid to
Z0.
Rapid to tool change position.
Activate tool 1, centerdrill.
Activate spot drill cycle 1.
Call subprogram 1.
Activate tool 2, twist drill.
Activate peck drill cycle.
Call subprogram 1.
Activate tool 3, end mill.
Activate cutter compensation.
Feed to XY position.
Retract move in Z.
Feed to cutting depth.
Cut top of part.
Cut right side of part (vectored
path).
Activate circular interpolation.
Make arc move.
Feed to X position (bottom of
part).
Return to start position (cut left
side of part).
Move off part in Y.
Retract move in Z.
Cancel cutter compensation.
Cancel tool offsets and tools.
Retract to Z home.
Move off in X.
End Main.
Subprogram.
(Continued…)
All rights reserved. Subject to change without notice.
17-April-04
5-67
CNC Programming and Operations Manual
P/N 70000487G - Ellipses, Spirals, Canned Cycles, and Subprograms
Table 5-41, Loop Programming Example (Continued)
Blk. #
N28
5-68
Block
G90 G0 X2 (X50.80) Y-.5 9Y12.7)
N29
N30
N31
N32
LOOP 5
G91 X.75 (X19.05)
END
G80 G90 T0 Z0
N33
N34
X-2 (X-50) Y2 (Y50)
M99
Description
Activate Absolute and Rapid
Modes. Move to first hole
location.
Repeat following moves 5 times.
Distance between holes.
End of loop.
Cancel drill cycle. Activate
Absolute, Raise Z.
Rapid to tool change position.
Return to main program.
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Program Editor
Section 6 - Program Editor
Activating the Program Editor
Program blocks are written using the Program Editor. The Program
Editor can be activated from the Manual screen, Program Directory, or
Draw Graphics.
When you activate the Program Editor, the selected program opens for
editing.
Activating Edit Mode from the Manual Screen
To activate the Edit Mode from the Manual screen:
1. With the appropriate program loaded, press EDIT (F3). The Edit
Screen activates and Ins (F3) highlights. See Figure 6-1.
Activating Edit Mode from the Program Directory
To activate the Edit Mode from the Program Directory:
1. Highlight a program in the Program Directory.
2. Press EDIT (F8). The Edit screen activates and Ins (F3) highlights.
Activating Edit Mode from Draw Graphics
To activate the Edit Mode from Draw Graphics:
1. Press Edit (F2). The Edit screen activates and Ins (F3) highlights.
X0 Y0
Figure 6-1, Edit Screen
All rights reserved. Subject to change without notice.
17-April-04
6-1
CNC Programming and Operations Manual
P/N 70000487G - Program Editor
You can write and edit programs from the Edit Screen. The Edit screen
provides the following options:
Program Name
The name of the program listed on the screen.
Cursor Location
Indicates where text will be inserted (Line:Column).
Soft Key Labels
These labels define soft key functions. Some soft
keys, when pressed, activate pop-up menus that
contain additional features.
(edited) Marker
The (edited) marker indicates that the program has
been edited and the edits have not been saved.
Marked Block
Highlighted block(s) to which the activated editing
feature (cut, paste, delete, etc.) will be applied.
Program Listing
Area of the screen where the program is listed.
Editing Soft Keys
The Edit screen contains fourteen soft keys, four of which are activated
by pressing the SHIFT key. See Table 6-1.
To activate any SHIFT soft key:
1. In Edit Mode, press SHIFT and then press the appropriate soft key.
Table 6-1, Editing Soft Keys
6-2
Soft Key
Label
F Key
Help
F1
Activates Edit Help Menu.
Del
F2
Deletes a single character located at the cursor.
Ins
F3
DelBlk
F4
Activates Insert Mode. Use to insert typed
characters at the cursor without overwriting the
existing text.
Deletes a single block located at the cursor.
PgUp
F5
PgDn
F6
MOVE
F7
EDITING
F8
Function
Returns the display to the previous page of the
Program Listing.
Advances the display to the next page of the
Program Listing.
Activates the Move Pop-Up Menu. Use this menu to
return to the beginning or advance to the end of a
line or program. The menu contains word and line
search features.
Activates the Editing Pop-Up Menu. Use this menu
to perform various editing functions within a single
program or between two programs. This includes
inserting and restoring (deleted) blocks. It also
includes cutting and pasting blocks within a program
or writing and reading blocks between programs.
(Continued…)
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Program Editor
Table 6-1, Editing Soft Keys (Continued)
Soft Key
Label
F Key
Function
MISC
F9
Exit
F10
UnDelBk
SHIFT + F4
FinNext
SHIFT + F7
ChaNext
SHIFT + F8
Quit
SHIFT + F10
Activates the Misc Pop-Up Menu. Use this menu to
record keystrokes, recall recorded keystrokes,
repeat programming commands, print the program,
or display or edit another program.
Closes the Edit screen and returns the CNC to the
Program Directory.
Restores deleted blocks. The CNC will restore up to
128 deleted blocks.
Advances to the next occurrence of the text specified
in the Find Word feature. The Find Word feature is
located in the Move Pop-Up Menu.
Advances to the next occurrence of the text specified
in the Find Word feature and changes the text to the
replacement text specified in the Find Word feature.
The Find Word feature is located in the Move PopUp Menu.
Returns the CNC to the Program Directory without
saving edits made to the Program Listing.
Marking Programming Blocks
For many editing features, you must mark the affected program blocks
before the edit is performed. To mark program blocks:
1. In Edit Mode, place the cursor at the beginning of the first block to be
marked.
2. Press EDITING (F8). The soft key highlights and the Editing Pop-Up
Menu activates.
3. Highlight Mark block, and press ENTER. The block is marked.
4. Use ARROW keys to mark the appropriate blocks.
Unmarking Program Blocks
1. In Edit Mode, press EDITING (F8). The soft key highlights and the
Editing Pop-Up Menu activates.
2. Highlight Mark block. Press ENTER. Previously marked blocks will
no longer be highlighted.
All rights reserved. Subject to change without notice.
17-April-04
6-3
CNC Programming and Operations Manual
P/N 70000487G - Program Editor
Saving Edits
The Program Listing displays edits as soon as they are made, but the
edits are not saved until you exit the Program Editor. If the program
contains unsaved edits, the (edited) Marker displays next to the Program
Name.
To save edits:
1. In Edit Mode, press Exit (F10). The CNC returns to the Program
Directory or Draw Graphics screen and saves all edits.
Canceling Unsaved Edits
If edits have not been saved, they can be canceled.
To cancel unsaved edits:
1. In Edit Mode, press SHIFT and then press Quit (SHIFT + F10).
2. The message WARNING: Program has been edited. Sure you
want to Quit? displays on the screen, and the soft keys change.
Press Yes (F1) to cancel edits and return to the Program Directory.
Press No (F2) to return to the Edit Mode.
Deleting a Character
To delete a character:
1. In Edit Mode, use ARROWS to place the cursor on the character you
want to delete.
2. Press Del (F2) to delete the character.
Deleting a Program Block
There are two ways to delete program blocks from a Program Listing.
q
Use the DelBlk (F4) soft key to delete blocks one at a time.
q
Use the BLOCK operations Delete feature to delete several blocks at
a time.
To delete a program block using the DelBlk (F4) soft key:
1. In Edit Mode, place the cursor on the program block to be deleted.
2. Press DelBlk (F4). The CNC deletes the block.
To delete program blocks using the BLOCK operations Delete feature:
1. In Edit Mode, mark the blocks to be deleted.
2. Press EDITING (F8). The soft key highlights and the Editing Pop-Up
Menu activates.
3. Highlight BLOCK operations. Press ENTER. The Block Operation
Pop-Up Menu activates.
4. Highlight Delete. Press ENTER. The CNC deletes the marked blocks.
6-4
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Program Editor
Undeleting a Block
You can restore deleted blocks with the Undelete Block feature. The
last block deleted is the first block restored. There are two ways to
restore a block.
To restore a block using the EDITING (F8) Pop-Up Menu:
1. In Edit Mode, place the cursor at the point where the restored block
will appear.
2. Press EDITING (F8). The soft key highlights and the Editing Pop-Up
Menu activates.
3. Highlight Undelete Block. Press ENTER. The last line deleted from
the program displays at the cursor.
To restore a block with the SHIFT soft key menu:
1. In Edit Mode, place the cursor where the restored block will appear.
2. Press SHIFT and then press UnDelBk (SHIFT + F4). The last line
deleted from the program is inserted at the cursor.
NOTE: Up to 128 consecutively deleted blocks can be restored.
Canceling Edits to a Program Block
Use the Restore Block feature to cancel edits made to a program block
and restore the block to its original form. The feature must be activated
before the cursor has been moved to another block.
To cancel edits to a program block:
1. In Edit Mode, place the cursor on the program block to be restored.
Press EDITING (F8). The soft key highlights and the Editing Pop-Up
Menu activates.
2. Highlight Restore Block. Press ENTER. The CNC cancels the edits
and restores the original block.
Inserting Text without Overwriting Previous Text
Use Ins (F3) to activate the Insert Mode. In Insert Mode, the CNC inserts
typed text at the cursor, without overwriting previously entered text.
To insert text into a program without overwriting previously entered text:
1. In Edit Mode, press Ins (F3).
2. Place the cursor where you want to insert the text. Enter the new
text. The new text is inserted at the cursor. The CNC does not
delete previously typed text as you type.
All rights reserved. Subject to change without notice.
17-April-04
6-5
CNC Programming and Operations Manual
P/N 70000487G - Program Editor
Inserting Text and Overwriting Previous Text
To insert text into a program while overwriting previously entered text:
1. In Edit Mode, press Ins (F3) to cancel the Insert Mode. The soft key
will no longer be highlighted.
2. Place the cursor where the text will be inserted. Enter the new text.
The new text is inserted at the cursor. The CNC deletes previously
typed text as you type.
Advancing to the Beginning or End of a Block
To advance to the beginning or end of a program block:
1. In Edit Mode, place the cursor on any block of the program. Press
MOVE (F7). The soft key highlights and the Move Pop-Up Menu
activates.
2. Highlight End of Block. Press ENTER. The cursor advances to the
end of the block.
– or –
Highlight Start of Block. Press ENTER. The cursor returns to the
beginning of the block.
Advancing to the First or Last Block of a Program
To advance to the first or last block of a program:
1. In Edit Mode, press MOVE (F7). The soft key highlights and the
Move Pop-Up Menu activates.
2. Highlight End of program. Press ENTER. The cursor advances to
the last block of the program.
– or –
Highlight Start of program. Press ENTER. The cursor returns to the
first block of the program.
Searching the Program Listing for Selected Text
Use Find Word and Find Next to search blocks for selected text. Enter
the text to be found.
To find all references of text in a program:
1. In Edit Mode, place the cursor at the beginning of the program. (Find
Word and Find Next search forward in the program only.)
2. Press MOVE (F7). The soft key highlights and the Move Pop-Up
Menu activates.
3. Highlight Find Word. Press ENTER.
6-6
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Program Editor
4. The message Enter Word to Find: displays on the screen. Enter the
text to be found. Press ENTER. The cursor advances to the first
occurrence of the text in the program.
5. To advance to the next occurrence of the text, press MOVE (F7).
The soft key highlights and the Move Pop-Up Menu activates.
6. Highlight Find Next. Press ENTER. The CNC advances to the next
occurrence of the text in the program.
7. Use this method to search for all occurrences of the text in the
Program Listing.
NOTE: You can also activate Find Next from the SHIFT soft key menu.
8. In Edit Mode, press SHIFT. The soft key changes. Press FinNext
(F7). This soft key performs the same function as Find Next in the
Move Pop-Up Menu. Each time you press the soft key, the CNC
advances to the next occurrence of the Find Word text.
Going to a Block of the Program Listing
Use Go to Block to move to any line in the Program Listing. Go to
Block operates independently of block numbering. Blocks can be
numbered sequentially by any increment (1, 5, 10...). Go to Block
counts the blocks of the program in increments of 1 (1 [starting block], 2,
3...). When the feature is activated, the CNC goes to the line number
specified by the user, regardless of how the blocks are numbered.
Block #
Line #
N10
Line 1
N20
Line 2
N30
Line 3
1. In Edit Mode, press MOVE (F7). The soft key highlights and the
Move Pop-Up Menu activates.
2. Highlight Go to Block.
3. The message Go to Block: displays on the screen. Type in the
appropriate line number. Press ENTER. The CNC places the cursor
at that line number.
All rights reserved. Subject to change without notice.
17-April-04
6-7
CNC Programming and Operations Manual
P/N 70000487G - Program Editor
Replacing Typed Text with New Text
Use Change word to replace selected occurrences of text. Enter the
appropriate text and the CNC searches the Program Listing for all
occurrences of the text. You can edit or skip each occurrence.
To edit selected occurrences of the typed text:
1. In Edit Mode, EDITING (F8). The soft key highlights and the Editing
Pop-Up Menu activates.
2. Highlight Change Word. Press ENTER.
3. The message Enter String to Change: displays on the screen.
Enter the text to be replaced. Press ENTER.
4. The message Change <<TEXT>> with: displays on the screen.
Type in the replacement text. Press ENTER. The CNC goes to the
first occurrence of the text in the program. The message Change
<<TEXT>> with <<REPLACEMENT TEXT>>? displays on the
screen, and the soft keys change.
5. The CNC finds each occurrence of the text in the program. For each
occurrence, you can choose one of the following features:
Yes
No
All
(F1)
(F2)
(F3)
Only
(F4)
STOP
(F9)
Inserts replacement text for highlighted text.
Highlighted text does not changed.
Inserts replacement text for highlighted text for all
occurrences.
Changes highlighted word and exits to Edit
screen.
Change word feature is deactivated.
6. Press Yes (F1) to replace highlighted text with replacement text.
Press No (F2) to leave text unchanged. When you press Yes (F1) or
No (F2), the CNC highlights the next occurrence of the search text.
Change Word deactivates when all occurrences of the text have been
found or if you press Only (F4) or STOP (F9). After Change Word is
deactivated, the message Change complete; [# of changes]
occurrences changed. displays. The CNC returns to the Edit Mode.
NOTE: The ChaNext (SHIFT + F8) soft key provides another way to
change text entered in the Change Word feature.
7. With Change Word deactivated, press SHIFT. The SHIFT soft key
menu activates.
8. Press SHIFT and then press ChaNext (SHIFT + F8). The CNC finds
the next occurrence of the text entered in the Change Word feature.
It replaces the text with the replacement text specified in the Change
Word feature.
6-8
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Program Editor
Scrolling Through the Program
In Edit Mode, press the up and down ARROWS to scroll up and down in
the Program Listing.
Paging through the Program
With long programs, it is convenient to move the Program Listing display
up and down a whole page at a time.
1. In Edit Mode, press PgUp (F5) to advance forward or press PgDn
(F6) to go backward in the program. The CNC advances or goes
back one page at a time.
Inserting a Blank Line
Insert a line at the cursor with the Insert Line feature. All subsequent
lines will be moved down one line in the program. To insert a blank line:
1. In Edit Mode, place the cursor where you want the blank line to
appear. Press EDITING (F8). The soft key highlights and the Editing
Pop-Up Menu activates.
2. Insert line is highlighted when the menu activates. Press ENTER. A
blank line is inserted at the cursor. You can type a new program
block on the line.
All rights reserved. Subject to change without notice.
17-April-04
6-9
CNC Programming and Operations Manual
P/N 70000487G - Program Editor
Abbreviating Statements
To access statements without typing the entire statement, enter an
abbreviation assigned to the statement and activate Expand key.
For conditional statements, the CNC displays the statement and waits for
you to enter the condition under which the statement will be activated.
Not all statements require you to enter a condition.
Table 6-1 lists statements to which you can apply
Expand key, and the abbreviation assigned to each statement. The
statements are displayed within brackets. These brackets do not appear
on the screen.
Table 6-2, Statement Abbreviations
Abbreviation
Statement
D
[DO]
[END]
E
[END] or [ENDIF] or [ELSE]
G
[GOTO]
I
[IF (_) THEN]
[ENDIF]
L
[LOOP]
[END]
P
[PRINT]
W
[WHILE (_) DO]
[END]
To generate a statement from an abbreviation:
1. In Edit Mode, type the abbreviation that corresponds to the conditional
statement. The cursor must be on the space after the abbreviation.
2. Press EDITING (F8). The Editing Pop-Up Menu activates.
3. Highlight Expand key. Press ENTER. The CNC generates the
statement on the screen.
4. If the cursor displays within parentheses (_), you must enter a
condition under which the statement will be activated. Type in the
condition, if applicable.
6-10
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Program Editor
Copying Program Blocks
NOTE: You can cut, save and paste blocks within a Program Listing.
The Cut, Save and Paste features do not work for copying and
pasting blocks between two different programs.
Copy one or more program blocks and place them elsewhere in the same
Program Listing. Table 6-3 describes two ways to copy program blocks.
Table 6-3, Copying Program Blocks
Method
Description
Mark and save blocks
Copies and stores marked blocks. Leaves
original blocks unchanged.
Mark and cut blocks
Copies and stores marked blocks. Deletes
original blocks.
To mark and save blocks:
1. In Edit Mode, place the cursor at the beginning of the first block to be
copied.
2. Mark the blocks to be copied.
3. Press EDITING (F8). The soft key highlights and the Editing Pop-Up
Menu activates.
4. Highlight BLOCK operations. Press ENTER. The Block Operations
Pop-Up Menu activates.
5. Highlight Copy. Press ENTER. The CNC saves the blocks in memory
and the original blocks remain in the Program Listing.
To copy program blocks and delete the original blocks:
1. In Edit Mode, place the cursor at the beginning of the first block to be
copied.
2. Mark the blocks to be copied.
3. Press EDITING (F8). The soft key highlights and the Editing Pop-Up
Menu activates.
4. Highlight BLOCK operations. Press ENTER. The Block Operations
Pop-Up Menu activates.
5. Highlight Cut. Press ENTER. The CNC saves the blocks in memory
and deletes the original blocks from the Program Listing.
All rights reserved. Subject to change without notice.
17-April-04
6-11
CNC Programming and Operations Manual
P/N 70000487G - Program Editor
Pasting Blocks within a Program
To copy blocks and paste them into another section of the program:
1. In Edit Mode, place the cursor where you want to paste the copied
blocks.
2. Press EDITING (F8). The soft key highlights and the Editing Pop-Up
Menu activates.
3. Highlight BLOCK operations. Press ENTER. The Block Operations
Pop-Up Menu activates.
4. Highlight Paste. Press ENTER. The CNC pastes the copied blocks
into the Program Listing at the cursor.
Recording Keystrokes
Use Record Keys to record keystrokes as they are typed. It is useful for
recording block sequences that are used in several areas of the program.
When you activate Record Keys, the keystrokes are saved in a part of
memory called the “macro buffer”. The Play keys feature recalls
recorded keystrokes.
To record keystrokes as they are typed:
1. In Edit Mode, press MISC (F9). The soft key highlights and the Misc
Pop-Up Menu activates.
2. Highlight Record Keys. Press ENTER.
3. If any data has been stored in the macro buffer, the message
Overwrite existing macro buffer? displays. If the message
displays, choose Yes (F1).
4. Type in the appropriate text. The CNC records the typed text.
5. Highlight Record Keys. Press ENTER to deactivate the Record Keys
feature.
NOTE: Information remains in the macro buffer until overwritten by new
data or until the Edit Mode deactivates.
Retrieving Recorded Keystrokes
Use Play Keys to retrieve recorded keystrokes and print them on the
screen. To retrieve recorded keystrokes:
1. In Edit Mode, press MISC (F9). The soft key highlights and the Misc
Pop-Up Menu activates.
2. Highlight Play Keys. Press ENTER. The CNC displays the recorded
keystrokes at the cursor.
6-12
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Program Editor
Repeating a Command or Key
NOTE: Use Repeat Command with other features. You should
understand how a feature works before duplicating it with
Repeat Command.
The Repeat Command feature performs the following functions:
q
Repeats activated commands
q
Repeats (single) typed character
To repeat a command or character:
1. In Edit Mode, press MISC (F9). The soft key highlights and the Misc
Pop-Up Menu activates.
2. Highlight Repeat Command. Press ENTER.
3. The message Enter Repeat Count: displays. Enter the number of
times the command will be repeated.
4. The CNC prompts you to Select command (key) To Repeat.
5. Select the command (or key) to be repeated. The CNC repeats the
command. The command is repeated the number of times entered
after the Enter Repeat Count: inquiry.
NOTE: The maximum repeat count is 99,999.
(Re)numbering Program Blocks
To number or renumber blocks in a program:
1. In Edit Mode, mark all the blocks in the program.
2. Press EDITING (F8). The soft key highlights and the Editing Pop-Up
Menu activates.
3. Highlight BLOCK operations. Press ENTER. The Block Operations
Pop-Up Menu activates.
4. Highlight Renum. Press ENTER. The soft key menu changes.
5. The CNC displays the message, Enter starting N#:. Enter a value
(1, 5, 10...). The CNC assigns the number to the starting block of the
program. Press ENTER.
6. The message Enter N# increment: displays. Enter an incremental
value (1, 5, 10...). The CNC uses the entered values to number the
program. The numbering sequence assigned to the listing starts at
the number assigned to the starting block. Subsequent block
numbers are assigned based on the incremental value entered (1, 2,
3…; 5, 10, 15…; 10, 20, 30…).
7. Unmark highlighted blocks.
All rights reserved. Subject to change without notice.
17-April-04
6-13
CNC Programming and Operations Manual
P/N 70000487G - Program Editor
Printing the Entire Program
NOTE: Use the Print program located in the Block Operations Pop-Up
Menu to print part of a program.
Use Print program, from the MISC Pop-Up Menu, to print an entire
program. The parallel printer connection is located on the computer
assembly. The machine builder determines the actual position.
To print an entire program:
1. In Edit Mode, press MISC (F9). The soft key highlights and the Misc
Pop-Up Menu activates.
2. Highlight the Print program. Press ENTER.
3. The message Print <<PROGRAM.G>>? displays. Press Yes (F1) to
print the program.
– or –
Press No (F2) to cancel the feature.
4. When Yes (F1) is pressed, the CNC prints the program. A status
screen displays containing the program name, the line, page and
number of copies being printed. At the completion of the print job, the
CNC displays a message and the soft keys change.
5. Press Continue (F10) to return to the Edit screen.
NOTE: Press Cancel (F9) to cancel the print job while the program is
printing.
Printing a Portion of a Program
NOTE: Use Print program, from the Misc (F9) Pop-Up Menu, to print
the entire Program Listing.
Use Print, from the BLOCK Operations Pop-Up Menu, to print part of a
Program Listing. Select one or more blocks from the Listing. The CNC
prints out the selected blocks.
1. In Edit Mode, mark all blocks to be printed.
2. Press EDITING (F8). The soft key highlights and the Editing Pop-Up
Menu activates.
3. Highlight BLOCK operations. Press ENTER. The Block Operations
Pop-Up Menu activates.
4. Highlight Print. Press ENTER. The soft key menu changes.
5. The message Print selected block? displays. Press Yes (F1) to
print the program, or No (F2) to cancel the feature.
6-14
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Program Editor
6. When you press Yes (F1), the CNC prints the selected program
blocks. A status screen displays containing the program name and
the line, page, and number of copies being printed. At the completion
of the print job, the CNC displays a message and the soft keys
change.
7. Press Continue (F10) to return to the Edit screen.
NOTE: Press Cancel (F9) to cancel the print job while the program is
printing.
Accessing the Most Recently Used Programs
Use Pick Program, from the MISC Pop-Up Menu, to access and display
any of the last ten programs opened in the Edit Mode. The feature lists
the programs in descending order, with the most recently opened
program at the top of the list. The currently open program will not appear
on the list.
To access and display any of the last ten programs opened in the Edit
Mode:
1. In Edit Mode, press MISC (F9). The soft key highlights and the Misc
Pop-Up Menu activates.
2. Highlight Pick Program. Press ENTER. The Pick program screen
activates.
3. Highlight a program. Press ENTER. The CNC replaces the current
Program Listing with the selected program.
Opening Another Program from the Program Listing
After final edits have been made to a program, use Edit Program to
open and edit another program from the Program Listing. To use Edit
program to open a program:
1. In Edit Mode, press MISC (F9). The soft key highlights and the Misc
Pop-Up Menu activates.
2. Highlight Edit program. Press ENTER.
3. The message Enter program name: displays. Enter the program
name.
4. If the current Program Listing has been edited, the message
Program <<PROGRAM>> has been edited. Save before LOAD?
displays. Press Yes (F1) to save the edits; press No (F2) to cancel
edits to the current Listing.
5. If Yes (F1) is selected, press ENTER. The CNC displays the entered
program.
NOTE: Blocks saved in memory can be pasted into another program.
All rights reserved. Subject to change without notice.
17-April-04
6-15
CNC Programming and Operations Manual
P/N 70000487G - Program Editor
Copying Blocks to Another Program
Use Write, located in the Block Operations Pop-Up Menu, to copy one or
more blocks to another program. If you are copying to an existing
program, select the program to which the copied blocks will be written.
The Write feature deletes any information currently in the selected
program and replaces it with the copied blocks. If you enter a new
program name, the CNC creates a file with the name you entered and
adds an .M extension. The copied blocks remain in the original program.
To copy blocks from one program to another:
1. In Edit Mode, mark all blocks to be copied.
2. Press EDITING (F8). The soft key highlights and the Editing Pop-Up
Menu activates.
3. Highlight BLOCK operations. Press ENTER. The Block Operations
Pop-Up Menu activates.
4. Highlight Write. Press ENTER. The soft key menu changes.
NOTE: Press Cancel (F9) to cancel the operation.
5. The message Write block as: displays. Enter the name of the
program to which the blocks are being copied. (You must enter the
entire program name or the CNC generates an error message.)
Press ENTER. The blocks replace the existing program.
NOTE: Write does not use or overwrite information in the buffer, where
cut and saved blocks are stored. When the Write feature is
used, the information in the buffer remains unchanged.
Copying an Entire Program into Another Program
Use Read, in the Block Operations Pop-Up Menu, to copy an entire
program into the displayed Program Listing automatically. The copied
program will appear at the cursor.
1. In Edit Mode, press EDITING (F8). The soft key highlights and the
Editing Pop-Up Menu activates.
2. Highlight BLOCK operations. Press ENTER. The Block Operation
Pop-Up Menu activates.
3. Highlight Read. Press ENTER.
4. The message Enter program to read: displays. Enter the name of
the program to be copied into the Program Listing. Press ENTER. The
CNC copies the entered program into the Program Directory at the
cursor. The message Block read from <<PROGRAM>> displays
indicating that the operation is finished.
6-16
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Program Editor
Including Comments in a Program Listing
Use an asterisk (*) to make comments within a Program Listing or to
mask all or part of a block from the CNC. When an asterisk is placed
before a string of text, the CNC ignores all the text to the right of and on
the same block as the asterisk. Table 6-4 shows various ways to use the
asterisk in a Program Listing.
Table 6-4, Comment Blocks
Commented Block
*N20 G1 X5 Z6
N30 …
N20 G1 *X5 Z6
N21 …
N10 G70 G90 G0 X0 Z0 T0
N20 T1 *FACE/TURN TOOL
All rights reserved. Subject to change without notice.
17-April-04
Ignored Text
CNC ignores the entire block. The
next block is executed.
CNC activates Linear Interpolation
(G1). Then, programmed move to
X5 Z6 is ignored. The next block is
executed.
Block N20 activates Tool #1. The
comment contains the type of tool
used.
6-17
CNC Programming and Operations Manual
P/N 70000487G - Edit Help
Section 7 - Edit Help
Edit Help provides diagrams and entry fields to program move types and
Canned Cycles. The following section describes how to activate a Help
Graphic Screen for a G-code command and type values in the
appropriate entry fields.
NOTE: To select menu items (2 through 9, +/-, or .), press the key
corresponding to the desired item, and press ENTER. Menu
items 2 through 9 correspond to the numeric keypad keys 2
through 9. Menu item +/- corresponds to the +/- key. Menu
item . corresponds to the period (.) key.
– or –
If you know the G-code, type the G-code that you want, and
press ENTER to go directly to the Help Graphic screen. This is a
short cut to the Help Graphic screen; you do not have go
through the menus.
Figure 7-1, Overview of the Edit Help Screens illustrates how to activate
the Scaling (G72) Help Graphic Screen.
To access the Scaling (G72) Help Graphic Screen:
1. In Edit Mode, open the appropriate program. Press Help (F1). The
Edit Help Menu activates.
2. In the Edit Help Menu, press 2 (Compensation). Press ENTER. The
Compensation Help Template Menu activates.
3. Press 6 (Scaling). Press ENTER. The Scaling Help Graphic Screen
activates.
NOTE: Most Help Template Menus contain some inactive menu items.
Inactive menu items contain no graphics and no item numbers.
4. Type the appropriate scaling factor for the G72 (Scaling) Canned
Cycle. Fill in ALL entry fields displaying 0.0000. All other entries are
optional. In the Scaling Help Graphic Screen, all fields are optional.
5. Press ENTER. The program block displays in the Input Box. Press
Accept (F8) or ENTER to insert the block in the program.
– or –
1. In the Main Edit Help Menu or Help Template Menu, type the G-code
that you want (for example, G72), and press ENTER to go directly to
the Help Graphic screen. This is a short cut to the Help Graphic
screen; you do not have go through the menus.
2. Go to Step 4 above.
All rights reserved. Subject to change without notice.
17-April-04
7-1
CNC Programming and Operations Manual
P/N 70000487G - Edit Help
PATHS
Figure 7-1, Overview of the Edit Help Screens
7-2
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Edit Help
Main Edit Help Menu
The Main Edit Help Menu (Figure 7-2) displays categories for which Help
Menus are available. Refer to Table 7-1 for a description of Main Edit
Help Menu features.
Table 7-1, Main Edit Help Menu Features
Feature
Description
Menu Item Number
Use this number to select a menu item.
Help Templates
Access help template menus for selected
move type or canned cycle. (Help template
menus access help graphic screens in which
you program move types and canned cycles.)
Program Listing
The program open for editing.
G-Code Listing
Lists and describes commonly used G-codes.
Not a complete listing. Refer to “G-Code
Listing.”
M-Code Listing
Lists and describes commonly used M-Codes
(Miscellaneous Functions). Not a complete
listing. Refer to “M-Code Listing.”
Input Box
Displays commands selected in the Edit Help
Menu. The CNC inserts the selected
commands at the block displayed in the Input
Box.
NOTE: Before you activate the Edit Help
Menu, place the cursor on the
program block you wish to edit. The
CNC will activate the Edit Help Menu
with the cursor located on that block.
Soft Keys
Labeled function keys below the liquid crystal
display (LCD). Press the labeled soft key
(F-key) to activate.
Modal G-Codes
Modal G-codes do not program actual moves.
Use these commands to change the feedrate,
Inch/MM Mode, Absolute/Incremental Mode or
Feed Per Revolution/Feed Per Minute Mode.
Refer to “Modal G-Code Box.”
All rights reserved. Subject to change without notice.
17-April-04
7-3
CNC Programming and Operations Manual
P/N 70000487G - Edit Help
PATHS
Soft Keys
Figure 7-2, Main Edit Help Menu
Help Template Menu
Help Template Menus (see Figure 7-3) access submenus of move types
or G-codes. Refer to Table 7-2, Help Template Menus for available
Template Menus.
HI-LITE
SCALING
Rapid
C0
Soft Keys
Figure 7-3, Sample Help Template Menu
7-4
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Edit Help
Table 7-2, Help Template Menus
Template
COMPENSATION
2
LINES
Description
Compensated Moves
q
Rotation
q
Scaling
Reference Table
Table 7-4, Compensation
Help Template Menu
Line Moves
Table 7-6, LINE Help
Template Menu
Arcs
Table 7-7, ARCS Help
Template Menu
Radius or Chamfer Moves
Table 7-8, RAD/CHAMFER
Help Template Menu Table
Moves Containing Multiple
Radius and/or Chamfer
Moves
Table 7-9, MULTIPLE Help
Template Menu Table
Pocketing Cycles
Table 7-10, POCKETING
Help Template Menu Table
Plunge Pocketing Cycles
Table 7-11, PLUNGE
POCKETING Help Template
Menu
Spirals, Ellipses, Facing,
Circular Profile, Rectangle
Profile
Table 7-12, PATHS Help
Template Menu
Drill and Tapping Cycles
Table 7-13, DRILL/TAP Help
Template Menu
3
ARCS
4
RAD/CHAMFER
5
MULTIPLE
6
POCKETING
7
PATHS
8
DRILL/TAP
9
All rights reserved. Subject to change without notice.
17-April-04
7-5
CNC Programming and Operations Manual
P/N 70000487G - Edit Help
Help Graphic Screens
Scale factor U
Select
Abort
Accept
Prev
Exit
Soft Keys
Figure 7-4, Sample Help Graphic Screen
7-6
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Edit Help
Edit Help Soft Keys
The Edit Help Menu contains the following soft keys. Refer to Table 7-3.
Table 7-3, Edit Help Menu Soft Keys
Soft Key
Label and
(Name)
Soft Key
Number
F1
(UP)
F2
(DOWN)
Text
F4
Select
F5
ReEdit
F6
Abort
F7
Description
Moves highlight to the next Help
Template.
Moves highlight to the previous Help
Template.
Switches the text shown in the center of
the Edit Help Menu between two
choices. The CNC displays either:
q The active program and input box;
– or –
q Instructions for using the Edit Help
Menu, when available.
Selects the highlighted menu item.
To edit an typed command (G-code or
canned cycle), place the cursor on the
appropriate block and press ReEdit
(F6). Once all the fields have been
edited, press Accept (F8).
Deactivates the Edit Help Menu and
returns you to the Program Listing.
NOTE: Press Exit (F10) to close the
Edit Help Menu and save
accepted edits.
Accept
F8
Exit
F10
All rights reserved. Subject to change without notice.
17-April-04
Inserts the block displayed in the Input
Box into the program.
Returns you to the Program Listing and
saves accepted edits.
7-7
CNC Programming and Operations Manual
P/N 70000487G - Edit Help
Edit Help Menu
Refer to Figure 7-3, Sample Help Template Menu. Help Template Menus
access submenus of move types or G-codes. Refer to Table 7-2, Help
Template Menus for available Template Menus. Each Help Template
Menu contains the following features:
Help Templates
Labeled graphic of canned cycle or other
command. Press the required menu item to
activate the corresponding help graphic screen.
(Help graphic screens contain instructions for
inputting commands into the program.) For
available help template menus, refer to
Table 7-2, Help Template Menus.
Menu Item
Number
Press the required menu item to activate the
corresponding help graphic screen.
NOTE: To select a menu item: Press the menu
item number, then press ENTER.
Program Listing
Listing of program being edited.
NOTE: Press TEXT (F4) to replace the
Program Listing with on-screen
instructions for the active Help Template
Menu. On-screen instructions may
contain a description of each menu item
or general instructions for Edit Help.
Input Box
Displays the block where the CNC will add
programmed canned cycles or other commands
to the program.
NOTE: Before you press Help (F1) to activate
the Edit Help Menu, place the cursor on
the block you want displayed in the
Input Box.
Soft Keys
Labeled function keys below the liquid crystal
display (LCD). Press the labeled soft key (F-key)
to activate. The Help Template Menus contain
the same soft keys as the Edit Help Menu, with
the following exceptions:
ReEdit (F6) is inactive in the Help Template
Menu. Prev (F9) is active. Press Prev (F9) to
return to the previous screen.
Modal G-Codes
7-8
Modal G-Codes do not program moves. These
commands switch the Rapid/Feed Mode, Plane,
Inch/MM Mode, Absolute/Incremental Mode.
Refer to “Modal G-Code Box.”
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Edit Help
Refer to Figure 7-4, Sample Help Graphic Screen. Use the Help Graphic
screens to type parameters for canned cycles or other commands. When
you close the help graphic screen, the CNC inserts the block into the
program.
Help graphics screens are available for templates listed in Table 7-2,
Help Template Menus.
Help graphic screen features include:
Menu Item
Number
Help Templates
On-Screen
Instructions
Input Box
Menu items 2 through 9 are inactive. To make a
new selection, insert or cancel the block for the
active Help Graphic screen.
The help templates displayed on the screen
remain inactive.
Press Abort (F7) to cancel the block and exit Edit
Help. Press Accept (F8) to accept the block and
return to the Main Edit Help screen. Press Prev
(F9) to cancel the block and return to the Help
Template Menu. Press Exit (F10) to insert the
block into the program and return to the Program
Listing.
On-screen instructions include a description of
the selected menu item (move, G-code or
Canned Cycle) being programmed, the entry
fields and graphic pertaining to the selected
menu item.
Displays the block where the CNC will add
programmed canned cycles or other commands
to the program.
NOTE: Before you press Help (F1) to activate
the Edit Help Menu, place the cursor on
the block you want displayed in the
Input Box.
Soft Keys
Modal G-Codes
All rights reserved. Subject to change without notice.
17-April-04
Labeled soft keys describe the functions of the
F-keys located on the console. The help graphic
screens contain the same soft keys as the Edit
Help Menu, with the following exceptions:
ReEdit (F6) is inactive in the Help Template
Menu. Prev (F9) is active. Press Prev (F9) to
return to the previous screen.
Modal G-codes switch the Rapid/Feed Mode,
Plane, Inch/MM Mode, and Absolute/Incremental
Mode. Refer to “Modal G-Codes Box.”
7-9
CNC Programming and Operations Manual
P/N 70000487G - Edit Help
Using Help Graphic Screens to Enter Program Blocks
The Program Editor displays help graphic screens, in which you write and
edit program blocks.
When the CNC activates a help graphic screen, its first entry field is
highlighted. A highlight indicates that you can type values in an entry
field or make the appropriate selection. Press ENTER to move the
highlight to the next entry field. In the last entry field of the help graphic
screen, press Accept (F8) or ENTER to add the block to the Program
Listing. Press the ARROWS to move the highlight between entry fields
without typing values. Press CLEAR to clear an entry field.
There are two types of entry fields:
q
Required entry fields
Contain 0.000. You must type a value for
operation of canned cycle or other command.
q
Optional entry fields
Blank. Entry optional.
If a required entry field is left blank, the CNC writes the block using the
0.0000 default. This may generate an error message when the program
runs.
Optional entry fields do not require a value. When left blank, a default
value or position is usually assumed.
You must remember to type: decimal points and negative signs where
needed. The CNC assumes a positive value if no negative sign is typed.
Press the (+/-) key to insert a negative sign.
Compensation Moves, Rotation and Scaling
Press the CLEAR key to clear an entry.
7-10
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Edit Help
Table 7-4, Compensation Help Template Menu
COMPENSATION
2
COMPENSATION
Templates and Parameters
COMP OFF
G40
2
Select the COMP OFF template, and press ENTER. Inserts
the G40 command into the Input Box.
Tool Radius Compensation
canceled. Refer to “Section 9 Tool Page and Tool
Management” for more
information on tool
compensation.
Tool Radius Compensation, leftof-path, activated. Refer
“Section 9” for more information
on tool compensation.
COMP LEFT
G41
Description
3
Select the COMP LEFT template, and press ENTER.
Inserts the G41 command into the Input Box.
COMP RIGHT
G42
Tool Radius Compensation, rightof-path, activated. Refer to
“Section 9” for more information
on tool compensation.
4
Select the COMP RIGHT template, and press ENTER.
Inserts the G42 command into the Input Box.
ROTATION
G68
5
Refer to “Axis Scaling (G72)” in
“Section 4” for parameters and
description.
SCALING
G72
Refer to “Axis Rotation (G68)” in
“Section 4 - Preparatory
Functions: G-codes” for
parameters and description.
6
All rights reserved. Subject to change without notice.
17-April-04
7-11
CNC Programming and Operations Manual
P/N 70000487G - Edit Help
Line Moves
Line moves can be vectored moves (motion in two axes, X and Y) or
straight-line moves (motion in one axis, X or Y). To program Line moves,
type values for angles, endpoints and/or radii that define the move.
Figure 7-5 shows the Line Help Template Menu, which contains the
available line moves.
Figure 7-5, LINE Help Template Menu
To activate the Line Help Template Menu and program a line move:
1. In Edit Mode, open the appropriate program. Press Help (F1). The
Edit Help Menu activates. Refer to Figure 7-2, Main Edit Help Menu.
2. From the Edit Help Menu, type 3, and press ENTER. The Line Help
Template activates.
3. Select the appropriate menu item #2 to 9, and press ENTER. The
appropriate Line Help Graphic screen activates.
4. Type the required values or settings in the entry fields on the screen.
Press Accept (F8) or ENTER to insert the program block into the
program.
7-12
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Edit Help
Endpoint and Angle Calculation
Given the X, Y, or XY endpoints, the CNC can calculate the missing
endpoint(s) for line or rapid moves. Define the move as part of a right
triangle with the components identified as in Figure 7-6.
Figure 7-6, Move Orientation
Refer to Table 7-5. The CNC can calculate move endpoints, given:
q
q
q
q
q
Angle and radius
X position and angle
Y position and angle
X position and radius
Y position and radius
Table 7-5, LINE Move Types
LINE Moves
Defined By
Straight Lines
An X or Y endpoint (menu item 2 or 3, respectively)
Vectors
q
An XY endpoint (menu item 4)
q
An angle measured from the Y-axis and X or Y endpoint (menu item 5
or 6, respectively)
q
An angle measured from the Y-axis and the arc radius (menu item 7)
q
The arc radius and an X or Y endpoint (menu item 9 or 8, respectively).
All rights reserved. Subject to change without notice.
17-April-04
7-13
CNC Programming and Operations Manual
P/N 70000487G - Edit Help
Table 7-6, LINES Help Template Menu
LINES
3
LINES
Templates and Parameters
Move Description
Tool moves in a straight line along the Xaxis.
X: X endpoint. Req.
Tool moves in a straight line along the
Y-axis.
Y
3
Y: Y endpoint. Req.
Tool moves along a vectored path from
the current location to the X, Y endpoint.
X/Y
4
All entries are required.
X: X endpoint.
Y: Y endpoint.
Tool moves along a vectored path from
the current location to the X endpoint.
All entries are required.
C: Angle from X-axis (3 o’clock = 0).
X: X endpoint.
Tool moves along a vectored path from
the current location to the Y endpoint.
ANGLE/Y
6
All entries are required.
C: Angle measured from X-axis (3 o’clock = 0).
Y: Y endpoint.
(Continued…)
7-14
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Edit Help
Table 7-6, LINES Help Template Menu (Continued)
LINES
3
LINES
Templates and Parameters
Move Description
Tool moves along a vectored path from
the current location to the endpoint.
ANGLE/RADIUS
7
C: Angle measured from X-axis (3 o’clock = 0).
R: Radius.
Tool moves along a vectored path from
the current location to the endpoint.
RADIUS/X
8
R: Radius.
X: X endpoint.
Tool moves along a vectored path from
the current location to the endpoint.
RADIUS/Y
9
R: Radius.
Y: Y endpoint.
Arcs
Refer to “Programming Concepts” in “Section 1 - Introduction” for
information on planes and arc directions. The CNC executes arcs in the
XY (G17) plane by default. For an arc in the XZ (G18) or YZ (G19)
plane, program the plane change before the arc move. After you make
all the required moves in the XZ or YZ plane, return the CNC to the XY
plane.
Refer to Figure 7-7, Endpoint Radius Arc Types. There are two arcs that
can intersect any two points: an arc with an included angle less than 180
degrees and an arc with an included angle greater than 180 degrees.
All rights reserved. Subject to change without notice.
17-April-04
7-15
CNC Programming and Operations Manual
P/N 70000487G - Edit Help
Included Angle
Less Than 180 Degrees
(Positive Radius Value)
Start
Point
Included Angle
Greater Than 180 Degrees
(Negative Radius Value)
Start
Point
End
Point
End
Point
Figure 7-7, Endpoint Radius Arc Types
To program an arc with an included angle of less than 180 degrees, type
a positive radius value. To program an Arc with an included angle of
greater than 180 degrees, type a negative radius value. The CNC
chooses which arc center to use, based on the sign of the typed value.
Refer to Figure 7-8 and Figure 7-9, Incremental Mode, Center-Angle Arc.
Specify the appropriate Absolute or Incremental Mode for the angle and
center point. The direction (Cw/Ccw) of the Arc and the sign (+/-) of the
angle control the path of the tool.
If the Z-axis starting and end positions differ, the arc will be a helix.
o
90
o
Absolute 60
Cw Tool Path
Ccw Tool Path
o
Center Point
(Absolute Position)
Position
0
Absolute Angle
Reference
Starting Point
(Present Position)
Figure 7-8, Absolute Mode, Center-Angle Arc
7-16
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Edit Help
Figure 7-9, Incremental Mode, Center-Angle Arc
Table 7-7, ARCS Help Template Menu
ARCS
4
ARCS
Template and Parameters
Move Description
Tool moves from the current location
along the arc to the programmed XY
endpoint.
RADIUS/END
2
All entries are required.
X: X endpoint.
Y: Y endpoint.
R: radius of arc.
CENTER/END
3
Tool moves from the current location
along the arc to the programmed XY
endpoint. Type the circle center
coordinates (I,J). Use Z and L (optional)
to produce helical interpolation.
All entries are required.
X: X endpoint.
Y: Y endpoint.
Z: End depth.
I: X Horizontal circle center.
J: Y Vertical circle center.
L: Number of loops.
(Continued…)
All rights reserved. Subject to change without notice.
17-April-04
7-17
CNC Programming and Operations Manual
P/N 70000487G - Edit Help
Table 7-7, ARCS Help Template Menu (Continued)
ARCS
4
ARCS
Template and Parameters
Move Description
Tool moves from the current location
along the arc to the programmed X
endpoint. Type the circle center
coordinates (I,J).
All entries are required.
I: X Incremental arc center.
J: Y Incremental arc center.
X: X endpoint.
CENTER/Y
5
Tool moves from the current location
along the arc to the programmed Y
endpoint. Type the circle center
coordinates (I,J).
All entries are required.
I: X Incremental arc center.
J: Y Incremental arc center.
Y: Y endpoint.
CENTER/ANGLE
6
All entries are required.
I: X arc center.
J: Y arc center.
C: Angle measured from X-axis (3 o’clock = 0).
ARC/LINE
7
Tool moves from the current location
along the arc to the calculated endpoint.
Type the circle center coordinates (I,J)
and an angle measured from the 3
o’clock position. The CNC calculates the
endpoint.
The CNC performs an arc move to the
tangent point of the line intersection and
then moves at the specified angle (C) to
the XY endpoint.
All entries are required.
Q: Radius.
C: Angle measured from X-axis (3 o’clock = 0).
X: X endpoint.
Y: Y endpoint.
7-18
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Edit Help
Table 7-7, ARCS Help Template Menu (Continued)
ARCS
4
ARCS
Template and Parameters
LINE/ARC
Move Description
The CNC performs a LINE move to the
tangent point of the ARC intersection
and then moves at the specified radius
to the XY endpoint.
8
All entries are required.
C: Angle measured from X-axis (3 o’clock = 0).
Q: Radius.
X: X endpoint.
Y: Y endpoint.
CNC performs an arc move into another
arc move. The first arc ends and the
second arc begins at the tangent point of
the two arcs.
ARC/ARC
9
All entries are required.
I: 1st Horizontal X center of the first arc.
J: 1st Vertical Y center of the first arc.
I: 2nd Horizontal X center of the second arc.
J: 2nd Vertical Y center of the second arc.
X: End Horizontal X endpoint.
Y: End Vertical Y endpoint.
All rights reserved. Subject to change without notice.
17-April-04
7-19
CNC Programming and Operations Manual
P/N 70000487G - Edit Help
Table 7-8, RAD/CHAMFER Help Template Menu
RAD/CHAMFER
5
RAD/CHAMFER
Templates and Parameters
RADIUS
Move Description
The CNC performs a LINE move to the
tangent ARC, moves around the arc and
then moves along the second LINE to the
XY endpoint.
2
All entries are required.
X: Horizontal midpoint. (Intersection of lines).
Y: Vertical midpoint. (Intersection of lines).
Q: Radius of arc tangent to two lines.
X: Horizontal endpoint.
Y: Vertical endpoint.
CHAMFER
3
The CNC performs a LINE move to the
intersecting CHAMFER, moves across the
chamfer and then moves along the second
LINE to the XY endpoint.
All entries are required.
X: Horizontal midpoint. (Intersection of lines).
Y: Vertical midpoint. (Intersection of lines).
E: Chamfer distance.
X: Endpoint in X.
Y: Endpoint in Y.
CORNER RAD
G59
4
CORNER CHAMF
G59
5
The CNC performs an automatic corner
rounding at all intersecting elements (lines,
arcs) with the specified radius. Refer to
“Modal Corner Rounding/Chamfering
(G59, G60)” in “Section 4 - Preparatory
Functions: G-codes” for parameters and
description.
The CNC performs an automatic corner
chamfer at all intersecting elements (lines,
arcs). Refer to “Modal Corner
Rounding/Chamfering (G59, G60)” in
“Section 4” for parameters and description.
(Continued…)
7-20
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Edit Help
Table 7-8, RAD/CHAMFER Help Template Menu (Continued)
RAD/CHAMFER
5
RAD/CHAMFER
Templates and Parameters
CANCEL
G60
6
Move Description
Cancels G59 Corner Rounding or Corner
Radius. Refer to “Modal Corner
Rounding/Chamfering (G59, G60)” in
“Section 4 - Preparatory Functions: Gcodes” for parameters and description.
Inserts a G60 command.
Multiple Move Commands
Figure 7-10 shows the Multiple Help Template Menu, accessed through
the Edit Help Menu.
Multiple moves enable you to program more than one move on a single
program block. The allowed combinations include line, arc and chamfer
moves, in various combinations, as follows:
q
Two consecutive line moves (menu item 2)
q
Line to arc to line moves (menu item 3)
q
Line to chamfer to line moves (menu item 4)
q
Line-arc to line-arc-line moves (menu item 5) line-chamfer to linechamfer-line moves (menu item 6)
q
Line-arc to line-chamfer-line moves (menu item 7)
q
Line-chamfer to line-arc-line moves (menu item 8)
MULTIPLE
Figure 7-10, Multiple Help Template Menu
Menu item numbers reference the Multiple Help Template used to
program the Multiple move described. Refer to Table 7-9, MULTIPLE
Help Template Menu for definitions and input instructions regarding these
moves.
All rights reserved. Subject to change without notice.
17-April-04
7-21
CNC Programming and Operations Manual
P/N 70000487G - Edit Help
To use the Edit Help Menu to program a Multiple move:
1. Refer to Figure 7-2, Main Edit Help Menu. In Edit Mode, open the
appropriate program. Press Help (F1). The Edit Help Menu
activates.
2. From the Edit Help Menu, type 6, and press ENTER. The Multiple
MULTIPLE
6
Help Template activates.
3. From the Multiple Help Template, type the menu item (#2 to 8) of the
Multiple move to be added to the Program Listing. Press ENTER. The
appropriate Graphic screen activates.
4. Fill in the entry fields on the screen. Press Accept (F8) or ENTER to
insert the block into the program.
Table 7-9, MULTIPLE Help Template Menu
MULTIPLE
6
MULTIPLE
Templates and Parameters
Move Description
DEFINITION
2
C: First angle measured from X-axis (3 o’clock = 0).
The CNC performs a line move
along the first angle to the
intersection of the second angle
and then continues along the
second angle to the specified XY
endpoint.
C: Second angle measured from X-axis (3 o’clock = 0).
X: Horizontal endpoint.
Y: Vertical endpoint.
The CNC performs a line move
along the first angle to the tangent
arc, moves around the arc and
then moves along the second
angle to the specified XY endpoint.
RADIUS
3
C: First angle measured from X-axis (3 o’clock = 0).
Q: Radius of tangent arc.
C: Second angle measured from X-axis (3 o’clock = 0).
X: Horizontal endpoint.
Y: Vertical endpoint.
(Continued…)
7-22
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Edit Help
Table 7-9, MULTIPLE Help Template Menu (Continued)
MULTIPLE
6
MULTIPLE
Templates and Parameters
CHAMFER
4
C: First angle measured from X-axis (3 o’clock = 0).
Move Description
The CNC performs a line move
along the first angle to the
intersecting chamfer, moves
across the chamfer, and then
moves along the second angle to
the specified XY endpoint.
E: Length of intersecting chamfer.
C: Second angle measured from X-axis (3 o’clock = 0).
X: Horizontal endpoint.
Y: Vertical endpoint.
RAD/RAD
5
C: First angle measured from X-axis (3 o’clock = 0).
Q: First radius of arc tangent to 1st and 2nd Angles.
The CNC performs a line move
along the 1st angle to the tangent
arc. After completing the arc, the
CNC moves along the 2nd angle to
the tangent of the 2nd arc. After
completing the 2nd arc the CNC
moves to the specified endpoint.
C: Second angle measured from X-axis (3 o’clock = 0).
X: Midpoint.
Y: Midpoint.
Q: Second radius of arc tangent to 2nd Angle and
endpoints.
X: Endpoint.
Y: Endpoint.
(Continued…)
All rights reserved. Subject to change without notice.
17-April-04
7-23
CNC Programming and Operations Manual
P/N 70000487G - Edit Help
Table 7-9, MULTIPLE Help Template Menu (Continued)
MULTIPLE
6
MULTIPLE
Templates and Parameters
Move Description
CHAMF/CHAMF
6
C: First angle measured from X-axis (3 o’clock = 0).
E: Chamfer length intersecting chamfer 1st and 2nd
angles.
The CNC performs a line move
along the 1st angle to the
intersecting chamfer. After
completing the chamfer, the CNC
moves along the 2nd angle to the
intersection of the 2nd chamfer.
After completing the 2nd chamfer
the CNC moves to the specified
endpoint.
C: Second angle measured from X-axis (3 o’clock = 0).
X: Midpoint.
Y: Midpoint.
E: Chamfer length intersecting 2nd angle and endpoints.
X: Endpoint.
Y: Endpoint.
RAD/CHAMF
7
C: First angle measured from X-axis (3 o’clock = 0).
Q: Radius of arc tangent to 1st and 2nd angles.
The CNC performs a line move
along the 1st angle to the tangent
arc. After completing the arc, the
CNC moves along the 2nd angle to
the intersection of the chamfer.
After completing the chamfer the
CNC moves to the specified
endpoints.
C: Second angle measured from X-axis (3 o’clock = 0).
X: Midpoint.
Y: Midpoint.
E: Length of intersecting chamfer between 2nd angle
and
endpoints.
X: Endpoint.
Y: Endpoint.
(Continued…)
7-24
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Edit Help
Table 7-9, MULTIPLE Help Template Menu (Continued)
MULTIPLE
6
MULTIPLE
Templates and Parameters
CHAMF/RAD
8
C: First angle measured from X-axis (3 o’clock = 0).
E: Length of intersecting chamfer between 1st and 2nd
angles.
Move Description
The CNC performs a line move
along the 1st angle to the
intersecting chamfer. After
completing the chamfer, the CNC
moves along the 2nd angle to the
tangent arc. After completing the
arc the CNC moves to the specified
endpoint.
C: Second angle measured from X-axis (3 o’clock = 0).
X: Midpoint.
Y: Midpoint.
Q: Second radius of arc tangent to 2nd angle and
endpoints.
X: Endpoint.
Y: Endpoint.
All rights reserved. Subject to change without notice.
17-April-04
7-25
CNC Programming and Operations Manual
P/N 70000487G - Edit Help
Table 7-10, POCKETING Help Template Menu
POCKETING
7
Pocketing
Templates and Parameters
FRAME
G75
2
3
CIRC. POCK.
G77
Canned cycle to machine a convex or concave mold
rotation. Refer to “Mold Rotation (G45)” in “Section 5”
for parameters and description.
7
Canned cycle to machine an elbow cavity or core. Refer
to “Elbow Milling Cycle (G49)” in “Section 5” for
parameters and description.
ELBOW
G49
8
DRAFT POCK.
G73
7-26
Canned cycle to machine an irregular pocket. Refer to
“Area Clearance (Irregular) Pocket Milling (G169)” in
“Section 5” for parameters and description.
6
MOLD ROT.
G45
Canned cycle to machine a rectangular. Refer to
“Rectangular Pocket Milling (G78)” in “Section 5” for
parameters and description.
5
AREA CLEAR
G169
Canned cycle to machine a circular pocket. Refer to
“Circular Pocket Milling (G77)” in “Section 5” for
parameters and description.
4
RECT. POCK.
G78
Canned cycle to machine a frame pocket. Refer to
“Frame Pocket Milling (G75)” in “Section 5 - Ellipses,
Spirals, Canned Cycles, and Subprograms” for
parameters and description.
Canned cycle to machine a hole. Refer to “Hole Milling
(G76)” in “Section 5” for parameters and description.
HOLE
G76
Move Description
Canned cycle to machine a draft angle pocket. Refer to
“Draft Angle Pocket Cycle (G73)” in “Section 5” for
parameters and description.
9
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Edit Help
Table 7-11, PLUNGE POCKETING Help Template Menu
PLUNGE POCK.
Plunge Pocketing
Templates and Parameters
Move Description
Select PLUNGE POCK. (+/-) from the Pocket Help
Template Menu. Select CIRC. POCK. (2). Use for
carbide tooling to plunge in Z (single-axis) to the
programmed depth. Refer to “Plunge Circular Pocket
Milling (G177)” in “Section 5 - Ellipses, Spirals, Canned
Cycles, and Subprograms” for parameters and
description.
Select PLUNGE POCK. (+/-) from the Pocket Help
Template Menu. Select RECT. POCK. (3). Use for
carbide tooling to plunge in Z (single-axis) to the
programmed depth. Refer to “Plunge Rectangular
Pocket Milling (G178)” in “Section 5” for parameters and
description.
All rights reserved. Subject to change without notice.
17-April-04
7-27
CNC Programming and Operations Manual
P/N 70000487G - Edit Help
Table 7-12, PATHS Help Template Menu
PATHS
Templates and Parameters
ELLIPSE
G05
2
Sets CNC to Elliptical Interpolation Mode, executed at the
current feedrate. Refer to “Ellipses (G5)” in “Section 5 Ellipses, Spirals, Canned Cycles, and Subprograms” for
parameters and description.
Sets CNC to Spiral Interpolation Mode. Refer to “Spiral
(G6)” in “Section 5” for parameters and description.
SPIRAL
G06
Move Description
3
Sets CNC to Facing Interpolation Mode. Refer to “Facing
Cycle (G170)” in “Section 5” for parameters and
description.
Sets CNC to Circular Profile Interpolation Mode. Refer to
“Circular Profile Cycle (G171)” in “Section 5” for
parameters and description.
Sets CNC to Rectangular Profile Interpolation Mode. Refer
to “Rectangular Profile Cycle (G172)” in “Section 5” for
parameters and description.
7-28
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Edit Help
Table 7-13, DRILL/TAP Help Template Menu
DRILL/TAP
9
DRILL/TAP
Templates and Parameters
Move Description
Basic drill canned cycle. Refer to “Spot Drilling (G81)” in
“Section 5 - Ellipses, Spirals, Canned Cycles, and
Subprograms” for parameters and description.
DRILLING
2
G81
Counterboring canned cycle. Refer to “Counterboring
(G82)” in “Section 5” for parameters and description.
Peck drilling canned cycle. Refer to “Peck Drilling (G83)” in
“Section 5” for parameters and description.
PECKING
4
G83
Tapping canned cycle. Refer to “Tapping (G84)” in
“Section 5” for parameters and description.
TAPPING
G84
5
Bi-directional boring cycle. Refer to “Boring, Bi-Directional
(G85)” in “Section 5” for parameters and description.
BORE/BI
G85
6
Uni-directional boring cycle. Refer to “Boring, Unidirectional
(G86)” in “Section 5” for parameters and description.
BORE/UNI
G86
7
CHIP BREAK
8
G87
FLAT BORE
G89
Chip break cycle. Refer to “Chip Breaker Peck Cycle
(G87)” in “Section 5” for parameters and description.
Flat bore cycle. Refer to “Flat Bottom Bi-Directional Boring
(G89)” in “Section 5” for parameters and description.
9
All rights reserved. Subject to change without notice.
17-April-04
7-29
CNC Programming and Operations Manual
P/N 70000487G - Edit Help
Table 7-13, DRILL/TAP Help Template Menu (Continued)
DRILL/TAP
9
DRILL/TAP
Templates and Parameters
Bolt hole circle. Refer to “Bolt Hole Circle (G79)” in
“Section 5 - Ellipses, Spirals, Canned Cycles, and
Subprograms” for parameters and description.
BOLT HOLE
G79
+
Hole pattern drill cycle. Refer to “Hole Pattern (G179)” in
“Section 5” for parameters and description.
PATTERN
G179
Move Description
.
Modal G-Code Box
NOTE: Refer to “G-Code Listing” in this section for more information on
programming G-codes in Edit Help.
Figure 7-11 shows the portion of the Edit Help Menu that displays Modal
G-Codes. Modal G-Codes define the way the CNC will interpret
commands.
Figure 7-11, Modal G-Codes
When the Edit Menu is activated, Rapid G0 is active. Press the ARROWS
to select Modal G-Codes. Press ENTER or Select (F5) to insert the
G-Code into the Program Listing.
7-30
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Edit Help
G-Code Listing
Refer to Figure 7-2, Main Edit Help Menu. The Main Edit Help Menu
contains a G-Code Listing. When a G-code is selected from the list, an
input screen activates. It contains instructions and entry fields that
pertain to the selected G-code. Use the screens to input G-codes. Refer
to Table 7-14.
Table 7-14, Most Common Modal G-Codes
G-Code
Rapid G0
Feed G1
CW Interpolation G2
CCW Interpolation G3
XY Plane G17
XZ Plane G18
YZ Plane G19
Inch G70
MM G71
Absolute G90
Incremental G91
Function
Axis moves made at rapidrate.
Axis moves made at feedrate.
Sets clockwise circular interpolation.
Sets counterclockwise circular interpolation.
Sets default plane.
Sets default plane.
Sets default plane.
Sets CNC to Inch measurements.
Sets CNC to MM measurements.
Sets CNC to Absolute Mode.
Sets CNC to Incremental Mode.
Entering a G-Code
To program a G-code from the G-Code Listing:
1. In the Main Edit Help Menu, highlight the G-Code Help Template
GENERAL
G
. Press ENTER. The G-Code Listing activates.
2. Highlight a G-code selection, and press ENTER. The CNC displays
input instructions and/or entry fields that pertain to the selected Gcode.
3. Highlight a G-code selection, and press ENTER. The CNC inputs the
selected G-code into the program.
– or –
The CNC prompts for any necessary values or setting selections.
4. Read any instructions provided on the screen. Fill in the entry fields.
5. Press Accept (F8) or ENTER. The CNC inputs the G-code into the
active Program Listing.
NOTE: If you type two G-codes that cannot be used on the same block,
the CNC generates an error message.
All rights reserved. Subject to change without notice.
17-April-04
7-31
CNC Programming and Operations Manual
P/N 70000487G - Edit Help
Table 7-15 describes the G-codes in the menu.
Table 7-15, Edit Help G-Code Menu
G-Code
Label and Description
G4
Dwell. Programs a timed or infinite dwell.
G9
Exact Stop (Single Block). Non-modal exact stop
check. Activates exact stop check for a single block.
G22
Stroke Limit. Activates/deactivates software limits.
G28
Reference Point Return. Return to Machine Home
directly or through an intermediary point.
G29
Return from Reference Point. Return from Machine
Home to the coordinates specified. (G29 Xn Zn)
G53
Fixture Offset(s). (Coor. Syst. Select) Shifts the
location of Absolute Zero to a preset location. The preset
location is the specified fixture offset, measured from
Machine Home and stored in the Fixture Offsets Table.
G61
Exact Stop Mode (Contouring Mode OFF). Modal
Exact Stop Check. Activates In-Position Mode.
G64
Contouring Mode (Exact Stop Mode OFF). Modal
Contouring Mode. De-activates In-Position Mode.
G65
Macro Call, Single (Non-Modal). Used in a program to
call a stored macro. Macros can be entered after the
main program (subprogram) or in another file (must use
file inclusion to call to active program). In non-modal
macro (G67) call, the variables can be changed at each
call.
G66
Macro Call, Modal. Used in a program to call a macro.
Macros can be entered after the main program
(subprogram) or in another file (must use file inclusion to
call to active program). In Modal macro (G66) call, the
variables will always contain the same values.
G67
Cancel Modal Macro. Cancels a G66 Modal Macro call.
G92
Preset Zero. Shifts the location of Absolute Zero to a
preset location. The preset location, measured from
Machine Home, is specified in the G92 command.
Entry Fields
When a G-code is selected from the G-Code Listing, instructions and
entry fields are listed on the screen. Type values for the required
parameters.
7-32
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Edit Help
M-Code Listing
Refer to Figure 7-2, Main Edit Help Menu. The Edit Help Menu contains
an M-Code Listing. You can program M-codes by selecting them from
the list. If the M-code requires a parameter, the software displays the
Help Graphic for the entered M-code. Only M30, M98 and M100 require
parameters. Fill in the entry fields for these M-codes. Press Accept (F8)
to insert the selected code in the block or Prev. (F9) to cancel.
For other M-Codes, select the code and press Accept (F8) to insert the
code in the block. Press Prev. (F9) to cancel.
Table 7-16 describes the M-Codes in the menu.
Table 7-16, Edit Help M-Code Listing
M-Code
M0
M2
M3
M4
M5
M8
M9
M30
M98
M99
M100
M105
M106
M107
All rights reserved. Subject to change without notice.
17-April-04
Function
Program stop.
End of program.
Spindle ON FWD.
Spindle ON REV.
Spindle OFF.
Coolant ON.
Coolant OFF.
Jump to new program.
Call subprogram.
End subprogram.
Mirror image.
Dry-run, all axes.
Dry-run, NO Z-axis.
Dry-run off (cancels M105 or M106).
7-33
CNC Programming and Operations Manual
P/N 70000487G - Edit Help
Entering an M-Code
To program an M-Code from the M-Code Listing:
1. In the Main Edit Help Menu, highlight the M-Code Help Template
. Press ENTER. The M-Code Listing activates.
2. Highlight an M-code, and press ENTER. The CNC inputs the selected
M-Code into the program.
– or –
The CNC prompts for any necessary values or setting selections.
3. Press Accept (F8) or ENTER. The CNC inputs the M-Code into the
active Program Listing.
NOTE: If you type two M-Codes that cannot be used on the same block,
the CNC generates an error message.
Typing in Address Words
You can manually type in most address words without exiting Edit Help.
Address words that can be typed into the program via Edit Help include:
dimension coordinates (XYZUW); spindle codes (S); feedrates (F); tool
codes (T); and preparatory codes (G). Use the following procedure:
1. From the Main Edit Help screen or from a Help Template Menu, type
the required commands. Edit Help displays the typed commands in
the center of the screen. If the address word requires a parameter,
the software displays an entry field in which you type the appropriate
value or selection.
2. Type the value or selection, if required. You can accept or cancel
commands just as you would in the Help Graphic Menus. Press
Accept (F8) to enter the block into the program. Press Prev (F9) to
cancel your entry and clear the screen. Accepted commands are
inserted in the program.
Example: Entering G-Codes
From the Main Edit Help screen, type G77, and press ENTER. The CNC
activates the Help Graphic for Circular Pocket Milling (G77).
7-34
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Edit Help
Typing in M-Codes
You can manually type in M-codes listed in the table. Refer to
Table 7-16, Edit Help M-Code Listing. Most of these M-codes (except
M30, M98 and M100) do not require additional parameter settings.
Press Accept (F8) to insert the entered M-code into the program.
For M-codes that do require additional parameter settings (M30, M98,
M100), Edit Help displays the Help Graphic for the M-code. Type the
required parameters and press Accept (F8) to insert the M-code into the
program.
1. From the Main Edit Help screen or from a Help Template Menu, type
the entire M-code. (Example: M2, M100, etc.) The Edit Help displays
the typed M-code.
NOTE: If the M-code requires a parameter, the software displays the
Help Graphic for the typed M-code. Only M30, M98 and M100
require parameters. Fill in the entry fields for these M-codes.
2. Press Accept (F8) to enter the block into the program. Press Prev
(F9) to cancel your entry and clear the screen. Accepted commands
are inserted in the program.
All rights reserved. Subject to change without notice.
17-April-04
7-35
CNC Programming and Operations Manual
P/N 70000487G - Viewing Programs with Draw
Section 8 - Viewing Programs with Draw
Draw Graphics (part graphics) is a method by which to prove a program
before you cut any material. It allows you to view the part edge and/or
tool path from different angles, zoom in on a particular area of the part
and generally, inspect the moves the machine is programmed to make,
without necessarily moving the axes. This reduces waste and the chance
of damaging a part.
The CNC has two Draw Modes: Draw Simulation Mode and Real-Time
Draw Mode. This section explains how to use Draw Simulation Mode to
view programs. It also explains how to set the display for a detailed
inspection of the programmed moves.
NOTE: Draw (lowercase letters with an uppercase D) refers to the
CNC’s Draw Simulation Mode; DRAW (all uppercase letters)
refers to the CNC’s Real-Time Draw Mode.
q
In Draw Simulation Mode, the CNC runs programs and simulates
machine movements in the viewing area. The machine does not
move.
q
In the Real-Time DRAW Mode, the CNC displays the machine moves
in the viewing area as it runs the program in Auto or Single Step
Mode.
Draw Simulation Mode soft keys change the viewing settings for both
modes. Refer to “Section 11 - Running Programs” for instructions on
how to run DRAW while cutting a part.
NOTE: You can change the display settings at any time in Draw
Simulation Mode. You cannot change the display settings in
Real-Time DRAW Mode.
When you select Draw (F7) from the Program Directory, Draw Simulation
Mode is activated. The CNC draws the part without machine movement.
When you start DRAW from Auto or S.Step Modes, Real-Time Draw
Mode is activated. The CNC draws the part while it is machining it.
Starting Draw
Draw Simulation Mode is started from the Program Directory. The
DISPLAY (F5) and Parms (F9) settings determine how Draw looks and
runs. You can make some changes from the soft keys while a simulation
is running. However, it is better to adjust viewing settings before starting
the simulation. In Draw Simulation Mode, the CNC does not hold the
operation of the program for Dwells and tool mounts.
All rights reserved. Subject to change without notice.
17-April-04
8-1
CNC Programming and Operations Manual
P/N 70000487G - Viewing Programs with Draw
To activate Draw Simulation Mode:
1. In the Program Directory, highlight a program and press Draw (F7).
The Draw graphic screen activates.
2. Press DISPLAY (F5). A pop-up displays. Fit highlights.
3. Press ENTER. Fit scales image to fit in the viewing area.
4. Press Run (F3). The soft key menu changes to display the available
simulation operation modes: Auto (F1), S.Step (F2), or Motion (F3)
and related settings.
Choose an operation mode:
q
Auto Mode runs the entire program without pause.
q
S.Step Mode executes the program one block at a time.
q
Motion Mode executes the program one move at a time, without
pausing on non-motion blocks.
5. Draw runs the highlighted program; the tool path is displayed in
viewing area and the machine remains idle.
Draw Screen Description
Information is displayed on the CRT. In the Status Area on the left side
of the screen, axis position, feedrate, tool number, and other status items
are displayed. Refer to Figure 8-1.
Soft Keys
Figure 8-1, Draw Simulation Mode
At the bottom of the screen, blocks of the program being run are
displayed if the display is set for Text ON. This setting is in the Parms
(F9) pop-up. Soft keys are also displayed.
8-2
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Viewing Programs with Draw
Programmed moves appear in four separate colors:
Rapid moves:
Dotted red line.
Feed moves:
Solid white line or arc.
Compensated moves:
Solid or dotted green, depending on feed
or rapid.
Drilled holes:
A yellow cylinder shows the programmed
diameter of the tools and the depth of the
hole(s).
Status items are represented as follows:
Blk:
Block Number currently being simulated.
X
X Current Position.
Y
Y Current position.
Z
Z Current Position.
F:
Currently active feed rate.
T:
Currently active tool number.
D:
Currently active tool diameter.
L:
Currently active tool length offset.
Loop:
Loop countdown, if loop is programmed.
Feed:
Type of current movement (rapid, feed, arc CW,
arc CCW).
View:
Graphics view (XY, XZ, YZ, ISO).
Comp:
Compensation setting (Both, Ignore or Use).
Mode:
Current operating mode: S.Step, Motion or Auto.
Start Thru End:
Range of block numbers to run in DRAW Mode.
4AX-DRL.G
Program Name.
Putting Draw in Hold
To pause Draw, press Hold (F8) or HOLD.
When Draw is in hold, press Start (F7) or START to continue.
Canceling Draw
To cancel the execution of a program in Draw Simulation Mode, press
Cancel (F9).
All rights reserved. Subject to change without notice.
17-April-04
8-3
CNC Programming and Operations Manual
P/N 70000487G - Viewing Programs with Draw
Draw Parameters
Viewing parameters are set two ways. Before the program is run, set the
parameters from the Parms (F9) Pop-Up Menu. Refer to Figure 8-2.
While the program is running, change the parameters from the soft key
menu. Some options appear in both places, some do not. Soft keys
switch the labeled feature ON or OFF. Active soft key features are
highlighted.
Figure 8-2, Draw Parameters Pop-Up Menu
Tool On or Off
When you run Draw with Tool On, a display shows the tool as it moves
through the part. A tool must be active and have a Diameter entered on
the Tool Page in order to be displayed. The size of the tool is scaled to
the tool’s Diameter. Draw runs faster with Tool Off.
[Default: On]
To switch Tool On or Off:
1. In Draw Mode, press Parms (F9). The Parameter Pop-Up Menu
displays.
2. Highlight Tool, and press ENTER. Tool switches between On and
Off.
3. Press Parms (F9). The Parms Pop-Up closes.
NOTE: Press Tool (F5) to change the Tool parameter while Draw is
running.
8-4
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Viewing Programs with Draw
Drawing Compensated Moves
The ToolComp setting controls if and how Draw handles compensated
moves. This allows you to see the effects of compensation on the moves
in a program. The Draw ToolComp setting does not affect program
execution.
There are three ToolComp options: )
q
Ignore a program’s compensated moves.
q
Use (display) a program’s compensated moves.
q
Both runs the program twice. (First without compensation then with
compensation.) The moves from both are displayed simultaneously.
Both is the only selection that allows a direct comparison between
compensated and uncompensated modes. [Default: Both]
To set the compensation parameter:
1. In Draw Mode, press Parms (F9). The Parameter Pop-Up Menu
displays.
2. Highlight ToolComp, and press ENTER. A pop up displays.
3. Highlight the desired selection, and press ENTER. The pop up closes.
4. Press Parms (F9). The Parms Pop-Up closes.
Showing Rapid Moves
Draw displays Rapid moves as dotted lines. You can turn off displayed
rapid moves to eliminate screen clutter. This parameter has no effect on
program execution. [Default: ON]
To switch Rapid On or Off:
1. In Draw Mode, press Parms (F9). The Parameter Pop-Up Menu
displays.
2. Highlight Rapid, and press ENTER. Rapid switches between ON and
OFF.
3. Press Parms (F9). The Parms Pop-Up closes.
NOTE: In Draw Mode, press Rapid (F6) to change the settings.
All rights reserved. Subject to change without notice.
17-April-04
8-5
CNC Programming and Operations Manual
P/N 70000487G - Viewing Programs with Draw
Setting Grid Line Type
Draw can display a two dimensional grid with dots or solid lines.
[Default: None]
To set the Grid parameter:
1. In Draw Mode, press Parms (F9). The Parameter Pop-Up Menu
displays.
2. Highlight Grid, and press ENTER. The Grid Pop-Up Menu displays.
3. Highlight the desired selection, and press ENTER. The Grid Pop-Up
closes.
4. Press Parms (F9). The Parms Pop-Up closes.
Setting Grid Size
The grid size is adjustable. The units are determined by the CNC’s
current mode. [Default: 1.00]
To set the Grid size:
1. In Draw Mode, press Parms (F9). The Parameter Pop-Up Menu
displays.
2. Highlight Grid size, and press ENTER. The CNC displays a number
entry field.
3. Type the desired size, and press ENTER. The new value is displayed
on the pop-up menu.
4. Press Parms (F9). The Parms Pop-Up closes.
Putting Draw in Motion, S.Step, or Auto Mode
Draw Simulation Mode executes programs three ways:
q
In Automatic Mode (Auto)
q
In Single-Step Mode (S.Step)
q
In Motion Mode (Motion)
In Automatic Mode, blocks are executed sequentially without pause until
the program is finished, the CNC is put in a hold, or an error stops the
program.
NOTE: Press Auto (F1) to switch to Automatic Mode.
In the Single Step Mode, one block of the program is executed each time
START is pressed. This allows you to run the program one block at a
time.
NOTE: Press S.Step (F2) to switch to Single Step Mode.
8-6
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Viewing Programs with Draw
In Motion Mode a program is executed from one motion to the next,
executing one motion each time START is pressed.
NOTE: Press Motion (F3) to switch the CNC into Motion Mode.
Select the default mode as follows:
1. In Draw Mode, press Parms (F9). The Parameter Pop-Up Menu
displays.
2. Highlight Mode, and press ENTER. The Mode Pop-Up Menu displays.
3. Highlight the desired mode, and press ENTER. The pop-up closes.
4. Press Parms (F9). The Parms Pop-Up closes.
NOTE: If you are using an offline keyboard and running Draw in Single
Step or Motion Modes, press SPACEBAR to continue the program
after each hold.
Automatic Draw Restart
The Run parameter determines whether Draw automatically restarts after
a DISPLAY setting change. This allows you to make more than one
setting change before you restart Draw.
Press Run (F3) to restart Draw when Run is OFF.
When Run is ON, Draw automatically starts after each DISPLAY change.
[Default: ON]
1. In Draw Mode, press Parms (F9). The Parameter Pop-Up Menu
displays.
2. Highlight Run, and press ENTER. Run switches between ON and
OFF.
3. Press Parms (F9). The pop-up closes.
Erasing the Draw Display
The Erase parameter sets Draw to clear the display when it starts a
program. When Erase is OFF, the old drawing remains in the viewing
area and new moves are drawn over it. [Default: ON]
Set the Erase parameter as follows:
1. In Draw Mode, press Parms (F9). The Parameter Pop-Up Menu
displays.
2. Highlight Erase and press ERASE. ERASE switches between ON and
OFF.
3. Press Parms (F9). The pop-up closes.
All rights reserved. Subject to change without notice.
17-April-04
8-7
CNC Programming and Operations Manual
P/N 70000487G - Viewing Programs with Draw
Running Draw for Selected Blocks
NOTE: Program blocks must have block numbers to use this feature.
Draw can run any part of a program or a subprogram. To run part of a
program, specify the Start N# and End N# block settings on the Parms
Menu. [Defaults: Start and End]
To run part of a subprogram, both the starting and ending blocks must be
within the subprogram. To run an entire subprogram select starting and
ending blocks that include the subprogram call from the main program.
If a starting block is inside a subprogram and the ending block is in the
main program, the CNC will stop and generate an Error message at the
end subprogram block because it cannot find the subprogram starting
block.
Starting Draw at a Specific Block
To start Draw at a specific block:
1. In Draw Mode, press Parms (F9). The Parameter Pop-Up Menu
displays.
2. Highlight Start N#, and press ENTER. The Start N# Pop-Up Menu
displays.
3. Highlight the desired selection, and press ENTER. If Start Of
Program is selected, Draw will start at the first block of the program.
If Other Block is selected, type the block number, and press ENTER.
4. Press Parms (F9). The pop-up closes.
Ending Draw at a Specific Block
To end Draw at a specific block:
1. In Draw Mode, press Parms (F9). The Parameter Pop-Up Menu
displays.
2. Highlight End N#, and press ENTER. The End N# Pop-Up Menu
displays.
3. Highlight the desired selection, and press ENTER. If End Of Program
is selected, Draw will stop at the last program block. If Other Block
was selected, type the block number, and press ENTER.
4. Press Parms (F9). The pop-up closes.
8-8
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Viewing Programs with Draw
Adjusting Draw Display
Draw has several display settings that allow you to customize the graphic
in the viewing window. Activate these settings from the DISPLAY (F5)
Pop-Up Menu. Refer to Figure 8-3.
Figure 8-3, Display Pop-Up Menu
Fitting the Display to the Viewing Window
Draw can automatically scale the display to fit into the viewing area.
To fit the display in the viewing area:
1. In Draw Mode, press Display (F5). A pop-up menu displays.
2. Highlight Fit, and press ENTER. The pop-up closes and the display
adjusts to fit into the viewing window.
Scaling the Display by a Factor
Draw can enlarge or reduce the display size by a factor.
To scale the Draw display:
1. In Draw Mode, press Display (F5). A pop-up menu displays.
2. Highlight Scale, and press ENTER. The pop-up closes and the CNC
prompts to enter the scale factor.
NOTE: Type a decimal number to reduce the size, type a whole number
to increase the size.
All rights reserved. Subject to change without notice.
17-April-04
8-9
CNC Programming and Operations Manual
P/N 70000487G - Viewing Programs with Draw
3. Type the desired factor, and press ENTER. The prompt disappears.
The next time Draw runs, the display will be scaled by the factor
entered.
Using the Window Zoom
Draw allows you to zoom in on any part of the display. Refer to
Figure 8-4.
Figure 8-4, DISPLAY Window (Zoom)
To zoom in on part of the display:
1. In Draw Mode, press Display (F5). A pop-up menu displays.
2. Highlight Window, and press ENTER. A window displays inside the
viewing window.
3. Use ARROWS to center the window over the area of interest.
4. Press Expand (F5) or Compress (F6) to increase or reduce the size
of the window.
NOTE: Press Reset (F7) to restore window to its original size. Press
Cancel (F9) to cancel the Window command.
5. Once the window is sized and positioned, press Enter (F10). The
window closes. The next time Draw is run, the part of the display
framed by the window will fill the viewing window.
8-10
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Viewing Programs with Draw
Halving Display Size
Draw can reduce the size of the display to half the existing size.
To reduce the display size by half:
1. In Draw Mode, press Display (F5). A pop-up menu displays.
2. Highlight Half, and press ENTER. The pop-up closes. The next time
Draw runs, the display will be half its present size.
Doubling Display Size
Draw can double the size of the display.
To double the size of the display:
1. In Draw Mode, press Display (F5). A pop-up menu displays.
2. Highlight Double, and press ENTER. The pop-up closes. The next
time Draw runs, the display will be twice its present size.
Changing the Viewing Area without Changing the Scale
To shift part of the screen in a desired direction without changing the
scale factor, use the Pan command. Refer to Figure 8-5. This is
especially useful on long parts that do not entirely fit in the Draw window.
Figure 8-5, DISPLAY Pan
All rights reserved. Subject to change without notice.
17-April-04
8-11
CNC Programming and Operations Manual
P/N 70000487G - Viewing Programs with Draw
When the Pan command is activated from the Display Pop-Up Menu, the
Pan line displays on the screen and the soft keys change. Press Start
(F5) to place the beginning of the Pan line (circle) on the part of the
screen to be shifted. Press End (F6) to point the End of the Pan line
(arrow) in the direction and distance the screen will be shifted.
To change the viewing area without changing the Scale factor:
1. In Draw Mode, press Display (F5). The Display Pop-Up Menu
displays.
2. Highlight Pan, and press ENTER.
3. The Pan line displays on the screen. Press Start (F5) and use
ARROWS to place the start of the Pan line (circle) on a part of the
screen.
4. Press End (F6) and use ARROWS to place the tip of the arrow to
indicate the appropriate direction and distance in which the view will
be shifted.
5. Press Enter (F10). The CNC shifts the selected part of the screen in
the selected direction.
NOTE: Press Reset (F7) to restore the graphic to its original size (size
when Pan selected). Press Cancel (F9) to cancel the Pan
command.
Erasing Display
To erase the display:
1. In Draw Mode, press Display (F5). The Display Pop-Up Menu is
displayed.
2. Highlight Erase, and press ENTER. The display is erased.
8-12
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Tool Page and Tool Management
Section 9 - Tool Page and Tool Management
The Tool Page stores data on tools, such as: tool number, diameter,
length offset, diameter wear, length wear, and tool type.
Functions of the Tool Page include: cursor movement, tool search, clear,
and calibrate. Refer to Figure 9-1.
Soft Key Labels
Figure 9-1, The Tool Page
Activating the Tool Page
Activate the Tool Page as follows:
1. Go to the Manual screen.
2. In the Manual screen, press TOOL (F9). The Tool Page activates.
All rights reserved. Subject to change without notice.
17-April-04
9-1
CNC Programming and Operations Manual
P/N 70000487G - Tool Page and Tool Management
Using the Tool Page
Press UP and DOWN ARROWS to highlight and select tool numbers (row
numbers). You can type tool information only in a highlighted row.
Highlight the appropriate row and type the values. The information on the
highlighted row is also displayed at the bottom of the screen (Active Row
Display) for easy reading. The cursor marks the location of information to
be typed.
Numbered rows correspond to tool numbers. When the CNC executes a
program block that activates a tool number, the values on that row of the
Tool Page are activated.
Press RIGHT and LEFT ARROWS to move from column to column. Tool
Page values are automatically converted to their inch or millimeter
equivalents when you change the CNC’s unit mode. Values must match
the CNC’s unit mode.
NOTE: The Tool Page is the only place where the CNC converts values
from Inch Mode to MM Mode, and vice-versa. Programmed
positions are not converted when you change the unit mode.
Press PgUp (F5) or PgDn (F6) to scroll through the tool table one page
at a time.
When you activate Tool #0, you cancel the active diameter and length
offset of the CNC. The Tool #0, Z0 position is usually set as the fully
retracted position of the quill.
All of the CNC’s Jog features can be run from the Tool Page. The
handwheels (if installed) can also be used.
The following features display on the Tool Page:
No.
Row Numbers link the values on a row of the Tool
Page to a tool number. A program block that
activates a tool number activates the values and
settings on that row of the Tool Page.
Position Display
Displays information regarding current machine
position and active Units Mode (Inch/MM).
Diameter
Tool diameter(s) applied when you activate tool
diameter compensation.
Length
Tool-length offset(s), which enable the CNC to
adjust the Z-axis position and position the tool tip.
Diameter Wear
Diameter wear offset(s), which compensate for
wear on the tool or an incorrectly sized tool.
Length Wear
Length wear offset(s), which compensate for wear
on the tool or an incorrectly sized tool.
Type
Press 1 or 2 to indicate a flat or end type mill,
respectively.
Active Row Display Displays the row on which the cursor is located.
Soft Key Labels
9-2
Identify the functions of the active soft keys.
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Tool Page and Tool Management
Finding Tools by Number
To find a specific tool number in the Tool Page:
1. Press Find (F4). The CNC displays the following prompt, Enter tool
number: and the cursor displays.
2. Type a tool number and press ENTER. The cursor moves to the
selected tool number.
Changing Tool Page Values
1. In the Tool Page, highlight the desired row. Position the cursor on the
desired column.
CAUTION: Ensure that the CNC is in the same unit mode, MM or
Inch, as the value you enter. To verify the unit setting,
look at the G-Code area of the Tool Page where either
G70 (Inch) or G71 (MM) is displayed.
2. Type the new value with all appropriate decimal values and press
ENTER (Or press any ARROW.). The value will be entered.
Clearing a Tool (Whole Row)
To clear a row:
1. In the Tool Page, highlight the row to be cleared.
2. Press ClrLine (F3). All values in the row return to zero.
Clearing a Single Value
To clear a single value:
1. In the Tool Page, highlight an entire row.
2. Position the cursor on the value you wish to clear and press
ALT + C. The value changes to zero.
Adjusting a Single Value
To adjust a single value:
1. In the Tool Page, highlight the desired row. Position the cursor on the
desired column.
2. Press the letter A key to display the message, “Enter adjustment
value.”
3. Type the amount of the adjustment. The adjustment value may be
positive or negative.
4. Press ENTER to adjust the value, and display the adjusted value on
the table.
All rights reserved. Subject to change without notice.
17-April-04
9-3
CNC Programming and Operations Manual
P/N 70000487G - Tool Page and Tool Management
Tool Page Soft Keys and Secondary Soft Keys
Press SHIFT while in the Tool Page to activate the secondary soft key
functions. Refer to Table 9-1.
Table 9-1, Tool Page Soft Keys and Secondary Soft Keys
Label
Soft Key
Soft Key Label and Function
Offsets
F1
ClrLine
F3
Enables entry to the G53 Offset pop-up
menu. Refer to “Section 4, Fixture Offsets
(Work Coordinate System Select), (G53).”
Clears the entire single line.
Find
F4
Enables “search” of a tool number
Page Up
F5
Moves the cursor one page backward
Page Down
F6
Moves the cursor one page forward
Calibrate Z
F8
Exit
F10
Inputs Z dimension (in reference to Machine
Home) into the highlighted length offset and
advances the cursor.
Exits the Tool Page and saves any changes.
ClrTabl
SHIFT + F3
Quit
SHIFT + F10
Clears the entire Tool Table after
confirmation.
Enables you to exit the Tool Page without
saving any changes that you have made.
T-Codes and Tool Activation
To activate a tool, program a T-code followed by the tool number. The
tool number corresponds to the row of the Tool Page that contains the
Tool-Length Offsets (TLOs) and other required values for the active tool.
Format: Txxxx
Format: Txx
Two-digit T-codes are used if the machine tool is not equipped with an
automatic tool changer (ATC). If the machine is equipped with an ATC,
then the four-digit T-code system can be used.
In the Txxxx format: The first two digits select the tool number (bucket in
the ATC from which the tool is retrieved); the last two digits select the
offset from the Tool Page. The CNC uses the last two digits as the active
tool number (whose offset is activated).
Examples:
T0101
T0207
T1210
T9999
T0100
9-4
Pick up tool from Bucket #1 and use Offset #1
ATC Bin #2 and Offset #7
ATC Bin #12 and Offset #10
ATC Bin #99 and Offset #99
ATC Bin #1 and CANCEL OFFSETS
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Tool Page and Tool Management
Tool Definition Blocks
Example: N3 T1 R1.25 L-1
A tool definition block defines the tool radius in the program, rather than
via the Tool Page. The block assigns Tool 1 a radius of 1.25 (diameter
equals 2.50).
Note: When using the Random Tool Replacement setting, the Tool Page
will have these differences:
q
A column headed Bin (displays the number of the bin that the tool is
in).
Bin T0: xx. Information in the top-right box of screen showing the bin
that holds the tool that is currently in use. The F2 soft key labeled
Bin T0 allows editing of this value.
q
A column headed Fix (Yes or No). When the cursor is in this column,
the bottom of the screen displays 1) YES 2) NO. Entering 1 or 2 will
display YES or NO in this column. If YES is displayed, then the tool
in that bin is always returned to that bin. If NO is displayed, then the
tool in that bin can be returned to another bin. The CNC software
automatically tracks the bins of tools that are returned to random bins.
Tool-Length Offsets
Tool-length offset (TLO) is the distance from Z0 Tool #0 to the tip of the
tool at the part Z0 (usually the surface of the work). Refer to Figure 9-2,
Tool-Length Offset.
Tool-length offsets allow each tool used in the part program to be
referenced to the part surface. In an idle state, the CNC does not have a
tool-length offset active. Therefore, Tool #0 (T0) is active. When T0 is
active, all Z dimensions are in reference to the Z Home position. When
you program T1, all Z dimensions become referenced to the surface on
which the tool-length offset was activated.
You must set the Z0 position of the quill. Usually, it is the fully retracted
position of the quill. Tool-Length Offsets are referenced to this position.
Because tools differ in length, Z0 axis (Part Zero) is not set the same way
as X0 or Y0. The tool-length offset is the distance from the tip of the tool
to the top of the part. Enter a length offset for each tool in the Tool Page.
All rights reserved. Subject to change without notice.
17-April-04
9-5
CNC Programming and Operations Manual
P/N 70000487G - Tool Page and Tool Management
Tool #0
Z 0.0
Part Zero
Figure 9-2, Tool-Length Offset
With tool-length offsets active, the Z-axis position display reads 0.00
when the active tool moves to Part Zero. Tool-length offsets simplify
programming.
Entering Offsets in the Tool Page
After you choose the type of tools and the order of their use in the
program, and you know the diameter and length offsets of tools, type the
data into the Tool Page.
1. In Manual Mode, press TOOL (F9) to open the Tool Page.
2. In the Tool Page, you must highlight a line before you can edit it.
Typically, you type diameter offsets in the Tool Page directly, after
measuring the tool with a micrometer.
To measure length offset:
1. In Manual Mode, put the tool in the spindle and carefully jog the tool
down until it touches surface (top of the work).
2. In the Tool Page, highlight that tool's tool number, and press Calib Z
(F8). This will take the dimension from Z Machine Home position, and
input it into the Length Offset column for that tool.
3. Exit the Tool Page, raise the Z-axis and continue.
– or –
Jog the tool(s) as described above, write down each offset(s) and
type it into the Tool Page.
9-6
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Tool Page and Tool Management
Setting Tool-Length Offsets
Before you run a job in production, perform the following steps:
1. Review the part drawing.
2. Make a machining plan. Include fixturing, tooling and machine
sequence.
3. Write the program on a program sheet.
4. Input the program.
5. Set the tool offsets.
The following sequence describes tool offsets for a job that center-drills,
drills and mills a part:
Tools:
#1
No. 3 center drill
#2
0.3750 diameter Twist drill
#3
0.5000 diameter End-mill
Typically, you would perform the following steps to activate TLOs:
1. Insert and tighten all tools in their appropriate holders.
2. Set the CNC to Manual Mode.
3. Type G28 Z and press START to home the Z-axis.
4. If the machine is a vertical knee mill, place the longest tool in the
spindle and raise the knee until the tip of the tool is approximately half
an inch from the top of the work.
5. Place Tool #1 in the spindle.
6. Jog the tool over the work.
7. Carefully jog the tip of the tool down to meet the top of the work. Use
MDI moves and/or the Manual Panel Jog selections.
8. Press TOOL (F9) to open the Tool Page.
9. Ensure that the cursor is on Tool #1 (row 1).
10. Press Calib Z (F8) to input the Z value in the Length column.
11. Press Exit (F10).
12. Raise the tool from the work to Z Home (Z0).
13. Repeat Steps 7 to 12 for all tools.
14. Use a micrometer to measure tool diameters and type those values in
their respective columns.
15. Press Exit (F10) to return to Manual Mode.
All rights reserved. Subject to change without notice.
17-April-04
9-7
CNC Programming and Operations Manual
P/N 70000487G - Tool Page and Tool Management
Entering the Z Position Manually
1. Retract the Z-axis to the Tool #0, Z0 position.
2. Load the tool and manually position its tip at the Part Z0 position.
3. Manually type the plus or minus Z position as it displays in the
position display. Press ENTER. Type the Z position in the offset
column.
NOTE: The value of a tool-length offset is usually a negative number.
Diameter Offset in Tool Page
When you activate a tool, you automatically activate the length offset and
diameter values recorded on the Tool Page. When a tool is activated, the
length offset is applied immediately to provide an accurate Z-axis position
display.
The active diameter value is important when you program compensated
moves and use cycles with built-in tool compensation. If tool diameter is
correct, compensated moves and cycles will be executed accurately too.
Enter tool-length offsets and tool diameter values on the numbered lines
of the Tool Page. The numbered lines on the Tool Page identify the tool
number (T-code) that activates those values.
You can program a tool activation as a separate block or include it within
the block for most moves and cycles. Tool activation’s programmed, as
separate blocks are easier to find in a Program Listing.
The Tool Page can store information for up to 99 tools.
On machines equipped with collet-type tool holders, it is impractical to
use the Tool Page to store tool-length offsets. You can set tool-length
offset at tool change. Tool Page diameters are still required for
compensated moves and when using cycles that have built-in
compensation. You can run all Jog features from the Tool Page.
Tool Page offsets activate when you program a T-code.
For example:
N3 T1
N4 G0 G41 XnYn
N5 etc...
Block N3 activates Tool #1 length offset. N4 activates tool compensation
for the following blocks.
NOTE: In Block N4, the G41 command must be accompanied by a
move (XYZ) to take effect. The motion must be in rapid (G0) or
feedrate (G1). The tool diameter activates when the CNC
executes the move programmed on the block. G40 and G42
must also be accompanied by moves, and activate in the same
manner.
9-8
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Tool Page and Tool Management
Tool Path Compensation (G41, G42)
NOTE: Be familiar with basic CNC principles before you attempt to write
compensated moves.
When tool compensation is not active, the CNC positions the tool’s center
on the programmed path. This creates a problem when programming a
part profile because the cutting edge is half a diameter away from the
path. Use tool diameter compensation to overcome this problem.
When tool compensation is active, the CNC offsets the tool by half a
diameter to position the cutting edge of the tool on the programmed path.
This enables you to program the coordinates along the part profile. You
do not need to adjust the path to compensate for tool diameter.
Most moves can be compensated. Specify right-hand or left-hand
compensation. "Right" or "left" refers to the side of the path to which the
tool offsets, as viewed from behind a moving tool. If the tool is to the left
of the work, use G41. If the tool is to the right of the work, use G42.
NOTE: Use tool compensation with lines and arcs only.
With left-hand tool diameter compensation (G41) active, the tool offsets
to the left of the programmed path (as viewed from behind a moving tool).
Refer to Figure 9-3.
Figure 9-3, Left Hand Tool Compensation
All rights reserved. Subject to change without notice.
17-April-04
9-9
CNC Programming and Operations Manual
P/N 70000487G - Tool Page and Tool Management
With right-hand tool diameter compensation (G42) active, the tool offsets
to the right of the programmed path (as viewed from behind a moving
tool). Refer to Figure 9-4.
Figure 9-4, Right Hand Tool Diameter Compensation
When the CNC encounters two consecutive, compensated moves, the
tool follows the offset path for the first move until it reaches the offset
path for the second move. The tool may intersect the offset path for the
second move, either before or after the endpoint of the first move,
depending on the geometry. Refer to Figure 9-5.
Move 2
Move 1
End Point
Tool Path
Move 1
COMP2
Figure 9-5, Consecutive Compensated Moves
The moves to and from compensated moves are called ramp moves.
Ramp moves give the CNC time to position the tool. The ramp move
must be at least half the active tool’s diameter in length. Refer to
Figure 9-6, Ramping into a Compensated Move.
9-10
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Tool Page and Tool Management
Workpiece
Offset path of
ramp intersects
offset path of cut.
Tool Starts Centered
On Ramp Move
Ramp move must be
at least 1/2 of a tool
diameter in length to
be effective.
First cut is a left hand
compensated Feed move.
(Programmed along
edge of workpiece)
Tool moves directly
to position perpendicular to
starting point.
Ramp move programmed
to starting point of first cut.
COMP5
Figure 9-6, Ramping into a Compensated Move
At the start of a ramp move, the tool centers on the programmed path. At
the end of the ramp move (starting point of the compensated move), the
tool centers perpendicular to the starting point, offset by half the tool’s
diameter.
When a compensated move starts and stops in a corner, the tool gouges
the work because the tool offsets to a position perpendicular to the
endpoint. Begin ramp moves at the side to avoid gouging the work.
Refer to Figure 9-7, Ramp On/Off Choices for Milling Inside a Square.
NOTE: Use canned cycles to cut profiles and pockets, when possible.
The CNC automatically selects Ramp On/Off positions in a
canned cycle.
All rights reserved. Subject to change without notice.
17-April-04
9-11
CNC Programming and Operations Manual
P/N 70000487G - Tool Page and Tool Management
Black Area Gouged
Ramp on
Position #1
Position #4
Ramp Off
Start
Position #2
Position #3
Poorly Chosen Starting & End Points.
Position #1
Position #2
Position #5
Ramp On And Ramp Off
Start
Position #3
Position #4
Preferred Method
COMP4
Figure 9-7, Ramp On/Off Choices for Milling Inside a Square
Using Tool Diameter Compensation and Length Offsets with Ball-End Mills
When you use a ball-end mill to cut contoured surfaces, use tool
diameter compensation and tool-length offset together, if at all. Unlike an
end tool, the tool-length offset for a ball-end mill is not set to the tip of the
tool.
Set the tool-length offset for a ball-end mill half the tool’s diameter back
from the tip. Refer to Figure 9-8, Setting Tool-Length Offset for Ball End
Mill.
9-12
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Tool Page and Tool Management
Ball End Mill
Quill At Tool# 0, Z 0 Position
1
_
2 Tool Diameter From Tip
Tool
Length Offset
Tool-Length
Offset Adjusted to
Adjusted
To Ball's Center
Ball’s Center
Part Zero
Figure 9-8, Setting Tool-Length Offset for Ball End Mill
Compensation (G40, G41, G42)
Cancel Mode in Tool Compensation: G40
At the end of a cutting sequence that performs tool compensation (G41
or G42), you must use G40 to cancel compensation. The following
example describes a part programmed in the XY plane using G41.
NOTE: You must make an X and/or Y move with or after G40, before
changing the active tool number.
Example:
N4
G17 G0 G41 Xn Yn
N5
etc...
.
.
N20
G0 G40 Xn Yn
N21
etc...
Program G40 on a line with G0 or G1 (unless G0 or G1 is already active).
G40 programmed with or immediately following G2 or G3 will generate an
alarm message.
All rights reserved. Subject to change without notice.
17-April-04
9-13
CNC Programming and Operations Manual
P/N 70000487G - Tool Page and Tool Management
Change of Tool Compensation Direction
It is possible, and sometimes advantageous, to change tool
compensation from G41 to G42, or from G42 to G41.
To change the direction of compensation, program the compensation
change with G0 or G1 in the motion to the new cutting position. After
outside milling with G41 (Move 1), program a G42 with the motion to the
new cutting position for the inside milling (Move 6). Refer to Figure 9-9.
G41
6
G42
2
G4
1
1
G4
CHANGEG41
Figure 9-9, Change of Tool Compensation Direction
Startup and Movement in Z Axis
The CNC “looks ahead” far enough to determine the next planar
intersection. Z-axis moves, even many consecutive Z moves, are
permitted at any time after a compensation block.
Refer to Example 1. N10 contains compensation block, properly
accompanied by an XY move. N11 contains a Z move.
Refer to Example 2. N10 contains the compensation block. N11 and
N12 contain two consecutive Z moves.
Example 1: Single Z move in a compensated program
9-14
N10
G0 G41 X0 Y-.5
N11
G1 Z-.125 F3
N12
Y3.625 F7.5
N13
X5.5
N14
etc...
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Tool Page and Tool Management
Example 2: Two Z moves in a compensated program
N10
G0 G41 X0 Y-.5
N11
Z.1
N12
G1 Z-.125 F3
N13
Y3.625 F7.5
N14
X5.5
N15
etc...
Temporary Change of Tool Diameter
To change the tool radius in order to leave stock for a finish pass,
program the "stock-variable". The variable assigned for this function is
#1030.
Example:
N120 #1030 = .015
When the CNC reads the above block, .015 will be added to the active
tool radius. The value in the Tool Page for that tool # will not be updated,
and tool compensation will be affected only until the tool is cancelled.
#1030 is temporary.
When the tool is cancelled (T0), #1030 is also cancelled.
Example:
N120 #1030 = -.015
In this case, .015 will be subtracted from the active tool's radius.
You must program the variable after the tool is activated.
You can program the variable regardless of whether G41 or G42 is
active. If compensation is not active at the time you program #1030, the
value will come into effect when compensation is activated.
#1030 is ignored for pocket canned cycles.
If compensation is active at the time the variable is read, the
compensation will go into effect immediately. The axis or axes will recompensate by making a move perpendicular to the next move
programmed in that plane (G17, G18, G19). Also, if the variable is read
with tool compensation active, you cannot program the variable directly
before or after an arc (it must occur between two linear moves in the
respective plane).
All rights reserved. Subject to change without notice.
17-April-04
9-15
CNC Programming and Operations Manual
P/N 70000487G - Tool Page and Tool Management
Motion of Tool During Tool Compensation
In linear-to-linear or linear-to-circular moves, the position at the end of the
startup block (block with G41 or G42) will be perpendicular to the next
programmed move in the plane. Refer to Figure 9-10 and Figure 9-11.
TOOL PATH
G41
PGM. PATH
G41PATH
Figure 9-10, A Linear-to-Linear Move
G41
TOOL PATH
PGM. PATH
G41LTOC
Figure 9-11, A Linear-to-Circular Move
In either case, the axes will move to a point perpendicular to the next
move during the startup block.
The length of the XY move that activates compensation must be equal to
or greater than the tool radius value. Example: If tool radius equals
.3750", the vector length of the XY move that activates compensation
must be .3750" or greater.
The same applies to the G40 (comp-off) move.
Refer to Figure 9-12, Paths During Tool Compensation. During tool
compensation, the CNC performs offset correctly and automatically.
Non-positioning moves such as dwells, coolant, or other auxiliary
functions are allowed. Moves in the third axis are also allowed during
compensation.
You cannot program a plane change (G17, G18 or G19) during tool
compensation. However, a 2-axis move off the currently active plane is
allowed.
9-16
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Tool Page and Tool Management
For example: G17 is the active plane (compensation in XY). You
program an XZ or YZ move. The Z-axis will reach the programmed
target as X/Y reaches its compensated target. Helical moves in the
active plane are also allowed. Do not program 3-axis moves during tool
compensation.
= INTERSECTING POINT
G41
G41
TOOL PATH
TOOL PATH
PGM. PATH
PGM. PATH
PATHS
Figure 9-12, Paths During Tool Compensation
Program G40 (cancel compensation) alone or with a move in the active
plane. The move must be in rapid (G0) or feedrate (G1). Deactivation
with G2/G3 is not permitted. The move must be at least the tool radius in
length.
The CNC "looks ahead" to following blocks in order to compensate
correctly. When it “sees” an upcoming G40 block, the CNC positions the
tool perpendicular to the last move before the G40 block.
Figure 9-13 shows tool movement as compensation is deactivated.
Figure 9-13, Offset Cancel
The tool moves to a point perpendicular to the last move before the G40
(deactivation) move.
All rights reserved. Subject to change without notice.
17-April-04
9-17
CNC Programming and Operations Manual
P/N 70000487G - Tool Page and Tool Management
Compensation Around Acute Angles
Refer to “Temporary Change of Tool Diameter” in this section. During
compensation, the CNC finds the compensated intersection of moves
and travels to that point.
On very sharp angles, this is not always desirable. For example, if you
compensate along the outside of a 15-degree corner angle, the
compensated intersection point will be far away from the actual point on
the work. Time is wasted by "cutting air" until the compensated point is
reached. To save time, the CNC creates an arc around the end of the
point on the work.
The CNC applies the arc where there are angles of 15 degrees or less.
This can be set in the Setup Utility or in the program. To change the
angle via program, set #1031.
Example: to change an angle to 10 degrees, program: #1031=10. Reprogram this value to 15 degrees (default) when finished.
The bottom part of Figure 9-14 shows how the CNC will automatically
"round" the compensated intersection. The work will remain a sharp
corner.
Actual Compensated
Intersection
Intersection
Automatically
Rounded
ACUTE
Figure 9-14, Compensation around an Acute Angle
9-18
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Tool Page and Tool Management
Change of Offset Direction
In Offset Mode, you can change the offset direction in special cases
without cancellation by G40. Refer to Figure 9-15 and Figure 9-16. The
change is not available in the startup block, in the block that follows it, in
the cancel block, or in the one previous to the cancel block.
The offset amount is assumed to be positive.
TOOL
PATH
G41
A
A
PGM.
PATH
TOOL
PATH
G42
PGM.
PATH
B
B
TOOL
PATH
A
B
G42
A = G42
B = G41
C
AT B, CHANGE TO G41
G42TO41
Figure 9-15, G42 to G41
G41
G41
G42
G42
G41
G42
PGM. PATH =
TOOL PATH =
G42_1
Figure 9-16, G42 to G41, Curved Paths
All rights reserved. Subject to change without notice.
17-April-04
9-19
CNC Programming and Operations Manual
P/N 70000487G - Tool Page and Tool Management
General Precautions
1. When you program tool path instead of part edge, a negative
diameter in the Tool Page effectively changes G41 to G42 in the
moves during compensation.
2. Third axis moves (not in the active plane) are permitted during
compensation.
3. The CNC automatically rounds off the compensated intersection of
acute angles of 15 degrees or less. To change this value, program
#1031.
4. It is possible to change the tool diameter currently in use with "stock"
variable #1030.
5. Startup (Ramp On) and cancellation (Ramp Off) blocks must be of G0
or G1 type, and must be at least the tool radius in length.
6. You must enter proper diameter value in the Tool Page before you
use tool compensation.
7. Compensated arcs must be on the active plane (G17 = XY, G18 =
XZ, G19 = YZ).
8. G53, G92 are permitted during compensation.
9. In Manual Mode, any active compensation deactivates.
10. Jog/Return is permitted during compensation.
11. System variable #1032 is available to change the number of blocks
the CNC can "look-ahead" while in tool-comp.
CAUTION: Changing this value can change the compensated tool
path. This variable enables further look ahead to prevent
undercut (excessive tool diameter). At default, the CNC
looks ahead far enough to find a valid intersection
between the current and next move. Set the variable
#1032 before you turn on the compensation (G40, G41
or G42).
9-20
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Tool Page and Tool Management
G41 Programming Example
Tool compensation can be activated with G41 or G42. Therefore you can
program the part-edge directly, rather than having to calculate the offset
manually. Refer to Figure 9-17 and Table 9-2. On a 3/8" diameter end
mill, the diameter value in the Tool Page for Tool #1 is .3750".
8"
(203.2mm)
7.5"
(190.5mm)
2.5"
(63.5mm)
5"
(127mm)
3"
(76.2mm)
.5" R
(12.7mm)
90 deg.
G41
Figure 9-17, Motion Example using G41: Absolute (G90)
Table 9-2, Motion Example Using G41
Standard
N1 O1010 * COMP-EX-1
N2 G90 G70 G0 T0 Z0
N3 X-3.0 Y1.0
N4 T1 * .375 MILL
N5 G41 X-.5 Y0
N6 Z.1
N7 G1 Z-.125 F5.0
N8 X8.0 F12.0
N9 X7.5 Y-2.5
N10 G3 X7.0 Y-3.0 I0 J-.5
N11 G1 X5.0
N12 X0 Y-2.5
N13 Y.5
N14 G0 Z.1
N15 G40 X-3.0 Y1.0
N16 T0 Z0
N17 M2
All rights reserved. Subject to change without notice.
17-April-04
Metric
N1 O1010 * COMP-EX-1
N2 G90 G71 G0 T0 Z0
N3 X-76 Y25
N4 T1 * 9.52 MILL
N5 G41 X-12 Y0
N6 Z2
N7 G1 Z-3.175 F125
N8 X203.2 F300
N9 X190.5 Y-63.5
N10 G3 X177.8 Y-76.2 I0 J-12.7
N11 G1 X127
N12 X0 Y-63.5
N13 Y12
N14 G0 Z2
N15 G40 X-76 Y25
N15 T0 Z0
N17 M2
9-21
CNC Programming and Operations Manual
P/N 70000487G - Tool Page and Tool Management
Refer to Table 9-3 for details on N-words.
Table 9-3, N-Codes and their Functions
N-Code
N1
N2
Function
Establishes program # and name.
Sets Absolute, Inch, Rapid; cancels tool offset, raises Zaxis.
Moves to tool change position.
Activates tool-length comp., also contains comment (*).
Activates tool diameter compensation and positions tool.
Positions Z above part.
Feeds Z to depth, at feedrate of 5.
Feeds first element of contour at new feedrate.
N9 to N13 feeds around contour.
Rapids Z above part.
Disables diameter compensation during rapid move to X3.0 Y1.0.
Cancels tool, moves Z to home position.
Ends program, resets CNC to N1.
N3
N4
N5
N6
N7
N8
N9
N14
N15
N16
N17
G42 Program Example
Refer to Figure 9-18 and Table 9-4, Milled Pocket Using G42 for an
example of a milled pocket created using G42.
5.5"
(139.7MM)
X0YO
2"
(50.8MM )
.5"
(12.7MM)
.5" (12.7 MM) ALL AROUND
G42
Figure 9-18, A Milled Pocket Using G42
9-22
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Tool Page and Tool Management
Table 9-4, Milled Pocket Using G42
Standard
N1 O1011 * COMP-EX-2
N2 G90 G70 G0 T0 Z0
N3 X-2 Y2
N4 T1 * .5000 MILL
N5 X1.5 Y-1.0
N6 Z.1
N7 G1 Z-.25 F5
N8 G42 X.5 F12
N9 G2 X1 Y-.5 I.5 J0
N10 G1 X5.0
N11 Y-1.5
N12 X1
N13 G2 X.5 Y-1 I0 J.5
N14 G40 G1 X4.7
N15 T0 G0 Z0
N16 X-2 Y2
N17 M2
All rights reserved. Subject to change without notice.
17-April-04
Metric
N1 O1011 * COMP-EX-2
N2 G90 G71 G0 T0 Z0
N3 X-50 Y50
N4 T1 * 12.7 MILL
N5 X38.1 Y-25.4
N6 Z2
N7 G1 Z-6.35 F127
N8 G42 X.5 F300
N9 G2 X25.4 Y-12.7 I12.7 J0
N10 G1 X127
N11 Y-38.1
N12 X25.4
N13 G2 X12.7 Y-25.4 I0 J12.7
N14 G40 G1 X119
N15 T0 G0 Z0
N16 X-50 Y50
N17 M2
9-23
CNC Programming and Operations Manual
P/N 70000487G - Tool Page and Tool Management
Table 9-5 describes N-Codes and their functions.
Table 9-5, N-Codes and their Functions
N-Code
N1
N2
N3
N4
N5
N6
N7
N8
N9 to N13
N14
N15
N16
N17
Function
Establishes program # and name.
Sets Absolute, Inch, Rapid, cancels tool offset, raises Zaxis.
Moves to tool change position.
Activates tool-length comp., block also contains comment
(*).
Positions to inside of pocket.
Position Z above part.
Feeds Z to depth at feedrate of 5.
Initiates compensation during feed move to arc start point.
N9 to N13 feeds around slot's contour.
Deactivates comp during move to clean-up center of pocket.
Cancels tool offset and rapids Z home.
Moves to tool (part) change position.
Ends program, resets CNC to N1.
Activating Offsets via the Program
In a program, T1 (by itself) calls the Tool Page diameter offset for the
specified tool. T1 with D, R, and L address words programs a temporary
diameter/radius and length offset independent of the Tool Page. The
entered D (diameter) or R (radius) and L (tool-length) offsets remain
active until you cancel the active tool. Refer to Table 9-6.
Table 9-6, Activating Offsets Using T1
T1 Format
T1
T1 D.5000 L-1.2500
T1 R.2500 L-1.2500
Description
Activates Tool #1 diameter offset listed in the
Tool Page.
Applies a diameter offset of .5000 and length
offset of -1.2500 to the active tool.
Applies a tool radius value of .2500 and
length offset of -1.2500 to the active tool.
The diameter offset takes effect when you program G41 or G42. All
dimensions are in reference to the work surface.
CAUTION: If you use T1 to activate a tool later in the program, the
Tool Page offsets for Tool #1 will be used (not the
values programmed via T1 Dn/Rn Ln).
NOTE: ANILAM recommends that you use the Tool Page to avoid
confusion or possible entry errors on the offsets.
9-24
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Program Management
Section 10 - Program Management
The Program Directory provides access to all of the program
management and floppy disk utilities. These functions include creating,
loading, deleting, restoring and copying programs. The Program
Directory also provides access to the floppy disk drives and the
communications utilities.
Press PROGRAM (F2) to activate the Program Directory from the Manual
screen.
The Program Directory’s USER listing lists the programs stored in the
CNC. Refer to Figure 10-1. All CNC programs have .G extensions after
their names. Change the display mode to view programs with other
formats.
Soft Keys
Figure 10-1, Program Directory
All rights reserved. Subject to change without notice.
17-April-04
10-1
CNC Programming and Operations Manual
P/N 70000487G - Program Management
Changing the Program Directory Display
You can change the Program Directory display to one of the following
modes:
q
Display only part program names (ending with .G extensions).
q
Display only part program names (ending with .G extensions) along
with size, date, and time of last edit.
q
Display all program names (ending with .G, .S, and .? extensions).
To change the Program Directory display mode, press Display
(SHIFT + F9). The display setting that shows only part program names is
usually the easiest to use.
Viewing All Programs of All Formats
To list all programs of all formats (including .G and .S):
1. In the Program Directory, press SHIFT. The soft key menu changes.
2. Press Log (F7). A pop-up displays.
3. Highlight Other, and press ENTER. The following prompt displays:
Log to:
4. Type *.*, and press ENTER. The CNC displays all programs of all
formats.
NOTE: To display only part programs, type *.G (part program
extension) at the prompt.
CAUTION: The Program Directory can provide access to internal
CNC programs. Tampering with internal programs can
cause the control to malfunction.
Creating a New Part Program
To create a new part program:
1. In Manual Mode, press PROGRAM (F2). The Program Directory
activates.
2. Press Create (F2). The control displays the prompt, NEW
PROGRAM: _.
3. Type the new program name.
4. Press ENTER. The new program name is inserted in the Program
Directory.
10-2
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Program Management
Choosing Program Names
A name cannot be longer than eight characters. If more than eight
characters are entered, only the first eight will be used. The CNC
displays program names in uppercase letters. No two programs can
have the same name. The CNC automatically places the .G extension
after the name.
Loading a Program for Running
You must load a program before you can run it. Only one program can
be loaded at a time.
To Load a program:
1. In the Program Directory, use ARROWS to highlight a program.
2. Press Select (F6). The CNC loads the program. The name of the
currently loaded program displays next to the SELECTED
PROGRAM label at the bottom of the screen.
Selecting a Program for Editing and Utilities
When the required program is highlighted, press Edit (F8) to activate the
Editor.
NOTE: If the Program Editor is activated in Manual Mode, the Editor will
open the loaded program.
To select a program for editing:
1. In the Program Directory, use ARROWS to highlight the program name.
2. Press Edit (F8). The Program Editor activates. The CNC displays
the listing for the selected program.
All rights reserved. Subject to change without notice.
17-April-04
10-3
CNC Programming and Operations Manual
P/N 70000487G - Program Management
Maximizing Program Storage Space
The CNC has a fixed amount of space available for program storage.
Use the System Information screen to check the availability of space.
Refer to Figure 10-2.
q
q
Total Space Available for the System is the total amount of
program storage space built into the CNC.
Total Free User Space is the available space for new programs.
6300M Off–Line
Figure 10-2, System Information Screen
When you run a program on the machine (or in Draw), the CNC
generates a second program of the same name followed by .S. The .S
programs contain information required by the CNC. Normally, an .S
program is larger than its associated part program. When you delete a
part program, the associated .S file is also deleted.
Periodically copy part programs to floppy disks for backup. ANILAM
recommends that you do not use the CNC for long-term storage of part
programs.
If many outdated programs are allowed to accumulate, the CNC could
run out of memory. To make room temporarily, delete the .S files of
programs that are not currently being used. The CNC will automatically
regenerate the .S files the next time the programs are run.
10-4
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Program Management
Displaying Program Blocks
List displays the blocks of a selected program. The displayed program
cannot be edited. The List feature only works on CNC part programs (.G
extension programs).
To list the contents of a program:
1. Select the program from the Program Directory.
2. Press List (F5). The CNC displays the program blocks and the List
Soft Key Menu activates. Refer to Table 10-1.
Table 10-1, List Feature Soft Keys
Soft Key
Label
Soft Key
Soft Key Label and Function
PgUp
F5
Scrolls backward through the Program
Listing one page at a time.
PgDn
F6
Home
F7
End
F8
Scrolls forward through the Program Listing
a page at a time.
Moves the cursor to the beginning of a
program.
Moves the cursor to the end of a program.
Find
F9
Exit
F10
Next
SHIFT
Enables you to search for specific text or
numbers in the program.
Returns you to the Program Directory.
+ F9
Finds the next occurrence of the Find
selection.
Deleting a Program
To delete a program:
1. Highlight a program in the Program Directory.
2. Press Delete (F3). The CNC prompts to confirm the deletion and the
soft keys change for your response.
3. Press Yes (F1). The CNC deletes the selected program.
– or –
Press No (F2). The Delete command is canceled.
NOTE: Deleting a program automatically deletes the associated .S file.
All rights reserved. Subject to change without notice.
17-April-04
10-5
CNC Programming and Operations Manual
P/N 70000487G - Program Management
Logging On to Other Drives
The Program Directory displays the programs in the C:\USER directory
by default. However, it can be set to show programs stored in other
drives or subdirectories. Press Log (SHIFT + F7) to activate the pop-up
menu. The pop-up lists the following choices: A:, C:, or Other. Select A:
to display programs stored on a floppy drive. Select C: to display user
part programs.
To list the programs in another drive or directory, choose Other. A
prompt displays. Enter the full pathname of the drive and directory
whose programs will be listed.
To display only the programs in a selected drive or directory:
1. In the Program Directory, press Log (SHIFT + F7). The Log Pop-Up
displays with the following selections: A:, C:, or Other.
2. Highlight Other, and press ENTER. The CNC displays the following
prompt: Log to:
3. Type the full pathname (including drive) of the directory, and press
ENTER. The CNC displays the programs stored in the specified
directory.
Marking and Unmarking Programs
You can perform some operations on more than one program at a time.
The Program Directory enables you to select (Mark) one, some or all of
the programs in the USER listing.
Marking Programs
To mark a program:
1. Highlight a program in the Program Directory.
2. Press ENTER. The marked program highlights and the highlight bar
advances to the next program.
3. Press ENTER to mark the next program.
– or –
Press ARROWS to highlight another program in the list, and press
ENTER.
4. Repeat these steps to mark as many program as required.
10-6
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Program Management
Unmarking Marked Programs
To unmark a program:
1. Highlight any marked program, and press ENTER. The program is no
longer marked.
Marking All Programs
To mark all programs in the Program Directory:
1. In the Program Directory, press Utility (F9). The Utility Pop-Up Menu
displays.
2. Highlight More, and press ENTER. The second page of the Utility
Pop-Up displays.
3. Highlight Mark All, and press ENTER. The CNC marks all programs in
the Program Directory. (Programs are highlighted.)
Unmarking All Marked Programs
To unmark all programs in the Program Directory:
1. In the Program Directory, press Utility (F9). The Utility Pop-Up
displays.
2. Highlight More, and press ENTER. The second page of the Utility
Pop-Up displays.
3. Highlight Unmark All, and press ENTER. The CNC unmarks all
programs in the Program Directory. (Programs are no longer
highlighted.)
Deleting Groups of Programs
1. From the Program Directory, mark all of the programs to be deleted.
2. Press Delete (F3). The CNC prompts to confirm the deletion and the
soft keys change for your response.
3. Press Yes (F1) to delete the selected programs.
– or –
Press No (F2) to cancel.
All rights reserved. Subject to change without notice.
17-April-04
10-7
CNC Programming and Operations Manual
P/N 70000487G - Program Management
Restoring Programs
A deleted program can be restored if the memory it occupied has not
been reused. Sometimes, only a portion of a deleted program can be
restored.
To restore a program:
1. From the Program Directory, press Utility (F9). The Utility Pop-Up
displays.
2. Highlight Restore, and press ENTER. If the CNC finds programs to
restore, it displays a pop-up menu. If the CNC does not find any
deleted programs, a No programs available for restore. message
displays.
3. When it finds deleted programs, the CNC lists them in a pop-up
menu. Highlight a deleted program, and press ENTER. The CNC
prompts for the first letter of the deleted program’s name.
4. Type the letter, and press ENTER. The CNC displays a message
indicating whether the program can be restored.
5. Press Cont (F10) to restore the program.
NOTE: Restored programs might not contain all of the original
information. Review any restored programs for accuracy before
you attempt to use them.
Copying Programs to Floppy Disks
Copy programs to floppy disks for storage or transfer to other machines.
To copy programs to floppy disks:
1. In the Program Directory, highlight the program or mark all programs
to be copied.
2. Press Utility (F9). The Utility Pop-Up Menu displays. Copy is
highlighted. Press ENTER. The Copy to: Pop-Up displays.
3. Highlight the target drive, and press ENTER. The CNC copies marked
programs to the target drive.
Renaming Programs
To rename a program:
1. In the Program Directory, highlight a program.
2. Press Utility (F9). The Utility Pop-Up displays.
3. Highlight Rename, and press ENTER. The CNC prompts: DEST.
PROGRAM:
4. Type new program name, and press ENTER. The new name replaces
the old name.
10-8
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Program Management
Printing Programs
The CNC can print to any standard IBM PC compatible printer. Use Print
to make paper copies of part programs. All marked programs are sent to
the printer.
To print one or more programs:
1. In the Program Directory, highlight the program or mark all the
programs to be printed.
2. Press Utility (F9). The Utility Pop-Up displays.
3. Highlight Print, and press ENTER. The CNC prompts to confirm the
command and the soft keys change for your response.
4. Press Yes (F1) to print the program(s).
– or –
Press No (F2) to cancel.
Checking Disks for Lost Program Fragments
Computer disks sometimes contain lost program fragments. This might
happen if a computer loses power while it is saving a program. Program
fragments do not appear in the Program Directory, but they take up
valuable program space.
To check for lost program fragments:
1. From the Program Directory, press Utility (F9). The Utility Pop-Up
displays.
2. Highlight More, and press ENTER. The second page of the pop-up
displays.
3. Highlight Check Disk, and press ENTER. The CNC prompts you to
select a drive.
4. Highlight the required drive, and press ENTER. The CNC checks the
disk. If lost clusters are found, the CNC prompts for recovery
instructions and the soft keys change for your response.
5. Press Yes (F1) to recover lost disk space; press No (F2) to cancel.
6. If you choose Yes (F1), the CNC attempts to recover lost disk space.
At the end of the procedure, press Cont (F10) to return to the
Program Directory.
All rights reserved. Subject to change without notice.
17-April-04
10-9
CNC Programming and Operations Manual
P/N 70000487G - Program Management
Displaying System Information
The System Information screen displays specific details about the CNC
and software package. Refer to Figure 10-3. Most information on this
screen is required only at setup or during troubleshooting.
6300M Off–Line
Figure 10-3, System Information Screen
To display the System Information screen:
1. In the Program Directory, press Utility (F9). The Utility Pop-Up
displays.
2. Highlight More, and press ENTER. The second page of the pop-up
menu displays.
3. Highlight System Info, and press ENTER. The System Information
screen displays.
Using Wildcards to Find Programs
The software supports the use of wildcards ? and * with the following
functions:
Copy ?
Rename ?
Print ?
Del ?
List ?
Load ?
NOTE: These functions are described in detail later in this section.
10-10
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Program Management
Table 10-2 describes the functions of the wildcards. For most functions
that support wildcards (except Del ?), when you include a wildcard in the
program name, the CNC displays a pop-up listing all filenames that
match your entry. Press the ARROWS to highlight a program from the list,
and then press ENTER to select that program.
When you use wildcards with the Del ? command, the CNC displays
each file matching the description in a separate pop-up. You can delete
or skip each program using labeled soft keys.
NOTE: Experiment with various wildcard formats to learn the most
efficient ways to use wildcards.
Table 10-2, Wildcard Examples
Wildcard
?
*
Function
Replaces
one
character.
Replaces
one or more
characters in
a filename.
You enter:
CNC displays a pop-up that:
?ROG.G
Lists all .G filenames
containing ROG preceded by
one character.
PROG?.G
Lists all .G filenames
containing PROG followed by
one character.
P??G.G
List all .G filenames
containing P--G with any two
characters between.
PR*.G
Lists all .G filenames starting
with PR and followed by other
character(s).
PROG.*
Lists all files named PROG
regardless of file format
(extension).
Lists all filenames starting
with PRO and followed by
other character(s) of any file
format (extension).
PRO*.*
All rights reserved. Subject to change without notice.
17-April-04
10-11
CNC Programming and Operations Manual
P/N 70000487G - Program Management
Copying Programs from/to Other Directories
Use Copy ? to copy programs to or from another directory, such as a
subdirectory or a floppy. Copy ? supports wildcards.
To copy programs to or from another directory:
1. In the Program Directory, press Utility. The Utility Pop-Up displays.
2. Highlight More, and press ENTER. The second page of the pop-up
menu displays.
3. Highlight Copy ?, and press ENTER. The CNC prompts for the name
and location of the source program.
4. Type the name and location (complete path) of the program, and
press ENTER. A pop-up prompts for the destination drive or Other
destination.
5. Highlight Other, and press ENTER. The CNC prompts for destination.
6. Type the new location (complete path), and press ENTER. The
program is copied into the new location.
Tip:
It is easier to log on to the floppy disk drive that contains the program,
mark the program and use the Copy to: feature.
Renaming Programs from/to Another Directory
Use Rename ? to rename programs in another directory, such as a
subdirectory or a floppy. Rename ? supports wildcards.
To rename a program in another directory:
1. In the Program Directory, press Utility. The Utility Pop-Up displays.
2. Highlight More, and press ENTER. The second page of the pop-up
displays.
3. Highlight Rename ?, and press ENTER. The CNC prompts for the
name and location of the source program.
4. Type the name and location (complete path) of the program to be
renamed, and press ENTER. The CNC prompts for new name and
location.
5. Type the new name and location (complete path) of the program, and
press ENTER. The CNC renames the program.
10-12
Tip:
The Rename ? feature can be used to move a program to a different
drive by entering a different program destination.
Tip:
Sometimes, it is easiest to log on to the floppy drive that contains the
program, mark the program and use the Rename ? feature.
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Program Management
Printing Programs from Another Drive/Directory
Use Print ? to print programs from another directory, such as a
subdirectory or a floppy. Print ? supports wildcards.
The CNC can print to any a standard IBM PC-compatible printer.
To print programs from another directory:
1. In the Program Directory, press Utility. The Utility Pop-Up displays.
2. Highlight More, and press ENTER. The second page of the pop-up
menu displays.
3. Highlight Print ?, and press ENTER. The CNC prompts for name and
location of source program.
4. Type the name and location (complete path) of the program to be
renamed, and press ENTER. The CNC prompts to confirm the
instruction and the soft keys change for your response.
5. Press Yes (F1) to send the program to the printer.
– or –
Press No (F2) to cancel the print job.
Tip:
Sometimes, it is easiest to log on to the floppy drive that contains the
program, mark the program and use the Print feature.
Creating Subdirectories
Press Sub Dir (SHIFT + F2) to create subdirectories. Ensure that the
CNC is in the desired drive before you create a subdirectory.
[Default: C:\USER]
To create a subdirectory:
1. In the Program Directory, press SHIFT.
2. The soft key menu changes. Press Sub Dir (F2).
3. The CNC prompts for the new subdirectory. Type the subdirectory
name, and press ENTER. The CNC creates the subdirectory.
All rights reserved. Subject to change without notice.
17-April-04
10-13
CNC Programming and Operations Manual
P/N 70000487G - Program Management
Deleting Programs on Another Drive
You can delete programs on another drive without logging on to that drive
via the Del ? (SHIFT + F3) command. The command supports wildcards.
To delete a program in another drive:
1. In the Program Directory, press SHIFT. The soft key menu changes.
2. Press Del ? (F3). The CNC prompts for the name of the program to
be deleted.
3. Type the name and location of the program (complete path), and
press ENTER. The CNC requests confirmation of the delete command
and the soft key menu changes for your response.
4. Press Yes (F1) to delete the program.
– or –
Press No (F2) to cancel the command.
Listing a Program in Another Drive/Directory
Press List ? (SHIFT + F5) to list a program in another directory. It
enables you to list programs in another drive without logging on to that
drive. Listing a program enables you to review the program without
editing it. The command supports wildcards.
The List ? (SHIFT + F5) soft key activates the same soft keys as List
(F5). Refer to “Displaying Program Blocks” in this section.
To list a program in another directory:
1. In the Program Directory, press SHIFT. The soft keys change.
2. Press List ? (F5). The CNC prompts for the name of the program to
be deleted.
3. Type the name and location of the program (complete path), and
press ENTER. The CNC displays the Program Listing for the entered
program.
10-14
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Program Management
Editing a Program in Another Directory
Press Edit ? (SHIFT + F5) to edit a program in another directory. You
can edit programs stored in another drive without logging on to that drive.
The command supports wildcards.
To edit a program in another directory:
1. In the Program Directory, press SHIFT. The soft keys change.
2. Press Edit ? (F5). The CNC prompts for the name of the program to
be deleted.
Type the name and location of the program (complete path), and
press ENTER. The CNC displays the Program Listing for the entered
program and activates Edit Mode.
Optimizing Your Hard Disk
When data is stored on a hard disk, it is stored in areas known as tracks
and sectors, similar to those on a CD. As more and more programs are
created, deleted, copied, renamed, etc., the hard disk becomes
fragmented. Information is stored in random unoccupied spaces.
Fragmentation slows down the performance of the hard disk. Therefore,
it will take longer to access information. To minimize fragmentation, you
must optimize your hard disk periodically. Your CNC has a built-in disk
optimizer. ANILAM recommends that you optimize your hard disk bimonthly, or at the very least, once every six months.
Accessing the Disk Optimizer
To access the Disk Optimizer:
1. In Manual Mode, press Program (F2). Press Utility (F9). A pop-up
displays.
2. Highlight MORE...., and press ENTER. The first entry in the window,
Disk Optimize highlights.
3. Press ENTER. The Optimizer automatically scans the hard disk
directories and examines the hard disk. This process takes up to
three minutes.
4. When the process is complete. A pop-up displays. You can Begin
Optimization or Exit Optimizer.
NOTE: Optimization is an automatic process; do not interfere with it
while it is running. If an emergency arises, press Cancel (F9) to
halt optimization.
5. The optimization process normally takes fifteen to ninety minutes,
depending on the size of the hard disk. To minimize run time,
optimize your hard disk as recommended.
All rights reserved. Subject to change without notice.
17-April-04
10-15
CNC Programming and Operations Manual
P/N 70000487G - Program Management
6. During optimization, the CNC displays the various processes that are
taking place.
7. When optimization is complete, the CNC displays: OPTIMIZATION
COMPLETE...Press any key to exit.
8. Press any key to return to the Program Directory.
10-16
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Running Programs
Section 11 - Running Programs
NOTE: Verify all programs in Draw before you run them. Refer to
“Section 8 - Viewing Programs with Draw.”
There are three modes of programmed operation:
q
Single-Step Mode
Runs a program one block at a time.
q
Motion Mode
Runs a program from motion to motion, without
stopping on non-move blocks (such as G41).
q
Automatic Mode
Runs a program automatically, without pausing.
The screens for all three modes resemble the Manual screen. Use the
soft key labels to distinguish between modes. The CNC highlights the
label for the active mode.
You must load a program before you can run it to cut a part. Load
programs from the Program Directory. Refer to “Section 10 - Program
Management” for information on how to load programs.
The Manual Data Input Mode (MDI) enables you to program a few quick
moves without having to create and save a program. MDI is usually used
for manual operation. It is available only in Manual Mode.
All programming tools, moves and cycles are available in MDI.
Refer to “Section 3 - Manual Operation and Machine Setup” for additional
information.
Running a Program One Step at a Time
The Single-Step screen accesses two execution modes: the Single-Step
Mode (S.STEP) and the Motion Mode (MOTION). Single-Step Mode runs
a program block by block; Motion Mode runs a program from motion to
motion. Both of these modes enable you to step through the program
and verify the moves before you cut an actual part.
Refer to Figure 11-1, Single-Step/Motion Screen. The S.STEP screen
looks like the Manual screen, but with fewer soft keys and S.STEP (F5)
highlighted.
To run a program in Single-Step Mode:
1. Go to the Program Directory, select a program and press Load (F6)
to load the required program.
2. Press Exit (F10) to return to the Manual screen.
3. In Manual Mode, press S.STEP (F5) to activate Single-Step Mode.
4. Press START to execute each block or motion.
NOTE: In Auto Mode, press S.STEP (F5) to activate Single-Step Mode.
All rights reserved. Subject to change without notice.
17-April-04
11-1
CNC Programming and Operations Manual
P/N 70000487G - Running Programs
Figure 11-1, Single-Step/Motion Screen
Active
Soft Key
(Highlighted)
Switching Between Motion and Single-Step Mode
Press MOTION (F7) to switch between Single-Step (S.STEP) and Motion
Mode (MOTION). When Motion Mode is active, MOTION (F7) highlights.
q
q
In Single-Step Mode, the CNC holds before it executes each block.
Press START to execute each block.
In the Motion Mode, the CNC holds before it executes each machine
move, but not before non-motion blocks. Press START to execute
each machine move.
Holding or Canceling a Single-Step Run
Press HOLD to halt the execution of the program. Press START to restart
a program that is on hold. Press MANUAL (F4) to cancel a program that
is on hold. When you cancel a program, the CNC terminates tool
compensation and canned cycles. All other modal settings remain active.
11-2
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Running Programs
Single-Step Execution of Selected Program Blocks
Using Arrows to Select a Starting Block
Select the starting block before you start program.
1. Load the required program and return to the Manual screen.
2. Press S.STEP (F5) to activate Single-Step Mode.
NOTE: To switch to Manual Mode, press MOTION (F7).
3. Highlight the desired starting block using the ARROWS.
4. Press START to execute the next block or motion.
Using SEARCH to Select a Starting Block
Use SEARCH to locate a specific block number or entered text. The
CNC highlights the first block found that contains the specified
information. SEARCH only searches forward in the program. Begin the
search from the starting block to search through the entire program.
1. From the Program Directory, load the required program and return to
the Manual screen.
2. Press S.STEP (F5) to activate Single-Step Mode.
3. Press SEARCH (F3). The CNC prompts for search number or text.
4. Type the required number or text, and press ENTER. The CNC runs
the search and highlights the first block it finds that contains the
number or text.
5. Press START to run the program from the highlighted block.
NOTE: After you start the program, it will execute normally.
Switching from Single-Step Mode to Auto Mode
To switch from Single-Step Mode to Auto Mode:
1. In Single-Step Mode, press AUTO (F6) to complete the current move,
then hold.
2. Press START to restart the CNC and run the rest of the program in
Auto Mode.
All rights reserved. Subject to change without notice.
17-April-04
11-3
CNC Programming and Operations Manual
P/N 70000487G - Running Programs
Position Display Modes
Position Displays for X, Y, Z, and U show:
q
Machine
Movement to the programmed (commanded)
position in reference to Machine Home.
q
Program
Movement to the programmed (commanded)
position in reference to Machine Home.
q
Target
The commanded position.
q
Distance to Go
Distance to go to reach the commanded position.
Automatic Program Execution
The Auto Mode is the CNC’s production mode. All or any part of a
program can be executed in the Auto Mode. Put the CNC in Auto Mode
from either the Manual or Single-Step Modes.
The Auto screen is similar to a Manual screen, but has fewer soft keys.
The AUTO (F6) soft key label highlights when the Auto Mode is active.
Refer to Figure 11-2.
To run a program in Auto Mode:
1. In the Program Directory, load the required program and return to the
Manual screen.
2. Press AUTO (F6) to activate Automatic Mode.
3. Press START. The CNC begins to execute program blocks.
Active Soft Key
(Highlighted)
Figure 11-2, Auto Screen
11-4
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Running Programs
Holding or Canceling an Auto Run
Press HOLD to halt the program. To restart a program on hold, press
START. To cancel a program that is on hold, press MANUAL (F4). The
CNC cancels any active tool compensation and canned cycles. Modal
settings (such as Absolute Mode or Inch Mode) remain active.
Starting at a Specific Block
Using Arrow Keys to Select Starting Block
1. From the Program Directory, select the required program and return
to the Auto screen.
2. Highlight the required starting block.
3. Press START to begin automatic program execution from the selected
block.
Using SEARCH to Select Starting Block
SEARCH directs the CNC to search the program for a block number, a
block that contains a number, or a block that contains specific text. The
CNC highlights the first block it finds that contains the search text.
SEARCH searches forward in the program until it reaches the end of the
program and then wraps to the beginning. Perform the search before
you run the program for production.
1. From the Program Directory, load the required program and return to
the Manual screen.
2. Press AUTO (F6) to activate Auto Mode.
3. Press SEARCH (F3). The CNC prompts for search number or text.
4. Type the number or text, and press ENTER. The CNC runs the search
and highlights the first block it finds that contains the number or text.
5. Press START to begin to execute the program from the highlighted
block.
NOTE: After you start the program, it will execute normally.
Clearing a Halted Program
When the CNC encounters a program block that generates an error, it
displays a Warning or error message and halts the program. Go back to
Manual Mode to correct the problem.
A program error could generate more than one message. Refer to
“Section 2 - CNC Console and Software Basics” for instructions on
reviewing undisplayed error messages.
After you correct the program, load and restart it at the appropriate block.
All rights reserved. Subject to change without notice.
17-April-04
11-5
CNC Programming and Operations Manual
P/N 70000487G - Running Programs
Using Draw while Running Programs
In Real-Time Draw, the CNC displays moves as it executes them. The
active S.Step (F5) or Auto (F6) highlights as does DRAW (F10). Refer
to Figure 11-3.
All display options in Draw Simulation Mode are available in the RealTime Draw Mode. Make all changes from Draw Simulation Mode before
you run the program.
NOTE: Press CLEAR to clear the Draw display.
To activate Draw while running a program.
1. Load the required program and put the CNC in S.STEP or AUTO
Mode.
2. Press DRAW (F10) to activate the Real-Time Draw screen and
change the soft keys.
3. Press START to run the program. The CNC displays moves as it
executes them.
Draw Real Time
and Operation Mode
Soft Keys
Figure 11-3, Draw (Real-Time Mode)
11-6
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Running Programs
Setting the CNC to Display an Enlarged Position Display
In the Manual, Auto, and S.Step Modes, you can set the CNC to display
an Enlarged Position Display. The Enlarged Position Display displays in
middle of the screen and shows motion to programmed positions. Refer
to Figure 11-4.
Active Soft Key
(Highlighted)
Fig11 epd
Figure 11-4, Enlarged Position Display
To switch the display between the Enlarged Position Display and the
default position display, in Manual Mode at the command line, type B,
and press ENTER.
To switch the display between the Enlarged Position Display and the
default position displays, in the S.Step/Auto Mode, press B.
Teach Mode
Use Teach Mode to input data to the program file from Manual Mode.
You can input axis positions, change modal status and input MDI
commands directly to the program.
A series of manual moves or positions can be made into a program, or
added to an existing program. Teach Mode is generally used to input
data when the desired tool position cannot be easily calculated. Jog
commands are also available in Teach Mode.
To store Teach Mode data in another program, you must create the
program first. You can also insert Teach Mode data into an existing
program.
All rights reserved. Subject to change without notice.
17-April-04
11-7
CNC Programming and Operations Manual
P/N 70000487G - Running Programs
Initiating Teach Mode
Select a program. In Manual Mode, press TEACH (SHIFT + F5) to put the
CNC in Teach Mode. After you press TEACH, Manual (F4) and TEACH
(F5) highlight, showing the active mode. The mode designator in the
upper-right area of the display indicates that Teach Mode is active. This
screen display is similar to the Auto and S.Step screens. The top area
will display the current program name with three lines of the program and
a highlighted command line (where data is typed and executed-stored),
and the mode of operation. The middle area will display the axes’
positions, target and distance to go (or Big number display). The bottom
area will display the CNC status.
The three lines of program shown will default to the first three blocks of
the current program. The COMMAND: line will be the third line. This
way, you can see the two previous and one subsequent block in case of
teaching moves into the middle of a program body. Press the UP/DOWN
ARROWS to move to a specific block. You can access Help (F1) at any
time.
Teach Mode Soft Keys
To activate the Teach Mode Soft Key menu, press TEACH (SHIFT + F5) in
Manual Mode. Refer to Table 11-1.
Table 11-1, Teach Mode Soft Keys
Label
Soft Key
Function
Help
F1
Activates Help.
Manual
F4
Activates Manual Mode.
Teach
F5
Activates Teach Mode.
Delete
F7
Deletes text.
Insert
F8
Inserts text.
Quit
F10
Exits Teach Mode and returns to Manual Mode
without saving changes.
In Teach Mode, TEACH (F5) highlights.
11-8
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Running Programs
Inputting Data with Teach Mode
In Teach Mode, the CNC can run data or store it. The highlighted block
denotes cursor position. If you input a move at that point, all subsequent
blocks will move down in the program structure. If you wish to add blocks
at the end of a program, press the ARROWS to move the cursor to the last
block in the program and input the blocks from there.
Press START (not ENTER) to input and activate MDI blocks into the
program.
Ways to store data include:
Command data G-codes, F-codes.
Axis data
XYZU positions.
1. If you type NO COMMAND or AXIS DATA in the command line and
press START, the CNC will store all axis positions with a G90 code
(and switch mode to G90, if necessary).
2. If you type NO AXIS or ONLY COMMAND in the command line and
press START, the command data will be stored with the axis positions
and a G90 code, and switch mode to G90, if necessary.
Example:
G1 F.007
When you type the above line in the command line and press START, that
information and the axes’ positions will be input into the program (with
G90). G91 will give error if used here.
3. If you type AXIS DATA WITH or WITHOUT COMMAND DATA on the
command line and press START, the block will be executed and stored
in the program simultaneously. The mode will change to G91, as
shown by active G-codes at bottom of screen. If axis data only is
typed, the current modals (G90-G91) will remain in use.
Example:
G91 G1 X1.5 F.005
All rights reserved. Subject to change without notice.
17-April-04
11-9
CNC Programming and Operations Manual
P/N 70000487G - Running Programs
Using Teach Mode
The positional data stored via Teach Mode is always referenced to the
current zero point (Program Zero).
1. Press ENTER to activate the following switch functions:
B Big (Large) number display
R Rapid override
P PLC status.
For example, press B + ENTER to switch to the large number display.
If you press START with no data on the command line, the CNC inserts a
G90 command with current axis positions.
If you press START with command data inputs, the CNC inserts a
command to move to the current axis positions and G90 code.
2. Press START to activate an axis or execute moves and inputs.
Command data is any data other than axis moves or locations. For
example, G-codes and F-codes.
Axis data is any axis move or location (such as X/Z).
The Handwheel (F10) soft key must be active before you initiate Teach
Mode. The handwheel cannot be turned on or off while in Teach Mode.
S, M, and T codes can be entered, but they will not be executed in Teach
Mode. They must be entered on a block by themselves.
No canned cycles can be executed in Teach Mode.
G91 will change the mode status, displayed at the bottom of the screen in
the active G-codes. Press START to activate G90.
To end the move without exiting Teach Mode, while a move is being
executed press Manual (F4).
Exiting Teach Mode
To exit Teach Mode and save changes to the program, press Manual
(F4). To exit without saving changes, press Quit (F10). The CNC
returns to Manual Mode.
11-10
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Running Programs
Parts Counter and Program Timer
The CNC keeps track of program run-time (TIMER) and the number of
completed parts (PARTS). The CNC displays Run-time in hours,
minutes, and seconds. These two features are available in the Manual,
Auto, and S.Step Modes. Refer to Figure 11-5.
TIMER
Number of
Completed Parts
Program Run
Time
Figure 11-5, Program Timer and Parts Counter
The Timer begins timing the program run when you press START and
stops when it encounters an M2 block. Therefore, ensure that an M2
block has been included at the end of the program.
The timer pauses if the CNC holds. The timer stops if you switch to
Manual Mode. If you re-run the program before going back to Manual,
the total time for all runs is displayed. The Timer values remain the same
until you switch to Auto or S.Step Mode again. Then, the timers reset to
zero.
The Parts counter starts at zero and increments by one every time the
CNC runs an M2 block. Therefore, ensure that an M2 block has been
included at the end of the program. The CNC continues to count parts
when you re-run the program in Auto or Single-Step. The parts counter
value is maintained when you switch to Manual Mode, but will reset to 0
when you switch back to Auto or Single-Step Mode. The Parts Counter
value can be modified via M-Codes. Refer to Table 11-2, M-Codes Used
with Parts Counter and Program Timer.
All rights reserved. Subject to change without notice.
17-April-04
11-11
CNC Programming and Operations Manual
P/N 70000487G - Running Programs
Table 11-2, M-Codes Used with Parts Counter and Program Timer
M-Code
M9355 X0
M9356 X0
M9376 Xx
M9377 Xx
11-12
Function
Prevents the parts counter from
resetting to zero.
Disables the Timer and Counter.
Presets any value into the parts
counter register. For example,
program M9376 X5 to preset 5 in
the parts counter register.
Adds entered number to the parts
counter. For example, if the current
parts counter value is 4 and you
then program M9377 X6, the new
parts counter value will be 10.
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Running Programs
Jog/Return
Jog/Return is a function in the CNC that allows the tool to be removed
from the cut while in Auto or S.Step Modes, without switching the CNC to
Manual. It has an ‘automatic return’ capability that will return the tool to
its departure point.
It is generally used to check to tool’s wear and to change a cutting
tool/offset in case of tool breakage or excessive wear in the middle of an
operation, or inspect a critical dimension or cut.
Initiating Jog/Return
The Jog/Return function may be initiated from the Auto or S.Step modes
of the CNC.
To use the Jog/Return feature, the HOLD key must be pressed first,
before pressing JOG (F9). This ensures that the machine cannot be
stopped accidentally while cutting by pressing JOG (F9). In this way, the
axes must be halted before the Jog/Return feature may be used.
Operations Allowed While “In” Jog/Return
Several motions/functions are allowed after the CNC has been put into
“Jog/Return”. The axes may be moved using the Manual Panel or by the
soft keys. Manual Date Input (MDI) moves are not allowed.
Any Tool-Length Offset can be changed while in Jog/Return mode.
Diameter offsets SHOULD NOT be altered with in Jog/Return mode (if
the current diameter offset is altered, the new value WILL NOT take
affect until the next time it is activated). ONLY THE CURRENT TOOL
LENGTH OFFSET should be altered with in this special mode. In this
way, if a tool breaks while in an operation, the user may replace the tool,
re-set the tool length offset, and “return” the tool to the cut without
aborting the program.
This is very useful and saves a great deal of time, if a tool breaks while in
the middle of a canned cycle or an extremely long cut.
All rights reserved. Subject to change without notice.
17-April-04
11-13
CNC Programming and Operations Manual
P/N 70000487G - Running Programs
Jog/Return Soft Keys
After the axes are halted by the HOLD key, and JOG (F9) is pressed, a
new strip of soft keys related to the Jog/Return function is displayed:
AUTOJOG
ZHOME
(F1)
Sends the axes to a pre-determined point, set by the
builder (in the Setup Utility)
Sends the axes to the HOME position
(F3)
MANUAL
(F4)
Cancels the Jog/Return mode, and sets the CNC to
Manual mode
RETURN
(F6)
Returns the axes to the position they were in when
Jog/Return mode was first entered into
COOL ON
(F7)
Turns the coolant ON
COOLOFF
(F8)
Turns the coolant OFF
TOOL
(F9)
Displays the CNC’s Tool Page
AUTOJOG (F1)
F1 (AUTOJOG) when pressed sends the axes to a pre-determined point,
set by the builder (in the Setup Utility). The default position is Machine
Home (X0, Y0, Z0, U0, W0). This is normally a position where a physical
tool change can be easily performed.
The order in which the axes retract to the pre-defined position is as
follows:
First:
Z retracts to home position
Second:
Y retracts to pre-defined position
Third:
X retracts to pre-defined position
Fourth:
U retracts to pre-defined position (if present)
Fifth:
W retracts to pre-defined position (if present)
Sixth
Z moves to pre-defined position
ZHOME (F3)
F3 (ZHOME) when pressed sends the axes to the HOME position. This is
a quick way to retract the tool from a cut, without hitting an overtravellimit switch. Z Home position is normally at the top of the Z travel.
WARNING: Check the Z display of MACHINE zero before pressing
this key.
MANUAL (F4)
F4 (MANUAL) when pressed cancels the Jog/Return mode, and sets the
CNC to Manual mode.
11-14
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Running Programs
RETURN (F6)
F6 (RETURN) when pressed returns the axes to the position they were in
when Jog/Return mode was first entered into.
The order in which the axes move to position is as follows:
First:
Z retracts to home position
Second:
Y returns to position
Third:
X returns to position
Fourth:
U returns to position (if present)
Fifth:
W returns to position (if present)
Sixth
Z returns to position
After all axes return to position, the machine will HALT, and the START
key must be pressed to continue the program.
COOL ON (F7), COOLOFF (F8)
F7 and F8 when pressed turn the coolant ON and OFF, respectively.
The coolant should be returned to its programmed status before F6
(RETURN) is pressed.
TOOL (F9)
F9 (TOOL) when pressed displays the CNC’s Tool Page. This allows the
operator to make a change to the CURRENT tool length or wear offset.
Only the CURRENT tool length or wear offset should be changed, as it is
the only value that will be invoked upon pressing RETURN (F6).
If the CURRENT tool length or wear offset is changed, the new value will
be invoked/activated with F6 (RETURN) is pressed. If any other values in
the Tool Page are changed, the new values WILL NOT be invoked until
that tool is (re-) activated at a later time.
HANDWHEEL (F10)
Enable or disables handwheel moves.
All rights reserved. Subject to change without notice.
17-April-04
11-15
CNC Programming and Operations Manual
P/N 70000487G - Running Programs
EXAMPLES:
The following are typical scenarios as to how and when to use the
Jog/Return function. Assume the CNC is running the program in Auto or
S.Step Modes.
SITUATION 1:
SITUATION1
Figure 11-6, Drilling Illustration
Refer to Figure 11-6. The tool is drilling in an X+ row of holes in a
workpiece. The tool becomes dull and breaks.
11-16
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Running Programs
Keystrokes/operations:
1.
HOLD
2.
JOG
3.
F3 (ZHOME) to raise Z
4.
Press SPINDLE OFF to stop spindle
5.
Press F8 (COOLOFF) to stop coolant
6.
Remove drill from holder
7.
Place new drill in holder
8.
Jog tool over workpiece with Manual Panel
9.
Jog tool down to offset surface
10.
TOOL
11.
CALIB Z
12.
EXIT
13.
Jog Z+ with Manual Panel [or press F3 (ZHOME)]
14.
Restart spindle by pressing SPINDLE FWD
15.
Restart coolant by pressing F7 (COOL ON)
16.
Press RETURN (F6)
17.
Press START to continue program
(F9)
(F9)
(F8)
(F10)
The axes will return to the position they were jogged from when the
Jog/Return function was initiated, in the described path.
SITUATION 2:
SITUATION2
Figure 11-7, Cutting Illustration
Refer to Figure 11-7. The tool is feeding along a Y– cut on the right side
of a workpiece. The tool becomes clogged with materials and is no
longer able to cut.
All rights reserved. Subject to change without notice.
17-April-04
11-17
CNC Programming and Operations Manual
P/N 70000487G - Running Programs
Keystrokes/operations:
1.
HOLD
2.
JOG
3.
F3 (ZHOME) to raise Z
4.
Press SPINDLE OFF to stop spindle
5.
Press F8 (COOLOFF) to stop coolant
6.
Remove end mill from holder
7.
Place new end mill in holder
8.
Jog tool over workpiece with Manual Panel
9.
Jog tool down to offset surface
10.
TOOL
11.
CALIB Z
12.
EXIT
13.
Jog Z+ with Manual Panel [or press F3 (ZHOME)]
14.
Restart coolant by pressing SPINDLE FWD
15.
Restart coolant by pressing F7 (COOL ON)
16.
Press RETURN (F6)
17.
Press START to continue program
(F9)
(F9)
(F8)
(F10)
The axes will return to the position they were jogged from when the
Jog/Return function was initiated, in the described path.
Notes on Jog/Return
q
q
q
q
q
q
q
q
11-18
Jog/Return is generally only used in trouble situations, where a tool
breaks or a tolerance must be checked. It allows the program to be
interrupted in AUTO or S.STEP mode, without having to switch to
Manual.
The HOLD key must be pressed prior to JOG.
Manual Panel moves are allowed while in Jog/Return.
Manual Data Input (MDI) moves are not allowed.
Tool length or wear offset on the CURRENT tool may be altered while
in Jog/Return. Care must be taken when updating offsets. The user
is responsible for entering to tool data correctly. The new CURRENT
tool length value will be in effect upon pressing RETURN.
If a limit switch is encountered, the CNC will cancel the Jog/Return
mode and switch to Manual mode.
The mode can be cancelled at any time by pressing F4 (MANUAL).
The Manual Panel is fully active (Handwheel also if present).
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - S and M Functions
Section 12 - S and M Functions
This section covers S and M code formats. Refer to Table 12-1. The
codes are included in the part program or activated in Manual Mode.
Table 12-1, S and M Codes
Code
S (Spindle)
M (Miscellaneous)
Function
Commands spindle speeds (S).
Performs miscellaneous (M) functions such
as spindle ON/OFF and coolant ON/OFF.
Speed Spindle Control (S-Function)
Format: Sxxx or Sxxxx
Spindle speed is programmed via S-code. The RPM range of the
machine determines the S-code range.
In determining spindle speeds there also may be gear ranges selected by
M-codes. For example, you may be able to select four ranges of speed
by programming the corresponding M-code for the required range. The
machine tool builder specifies the range. Refer to Table 12-2.
Table 12-2, M-Function Selected Ranges
M-Code
M40
M41
M42
M43
M44
Range Selected
Open gear range
1st Gear range
2nd Gear range
3rd Gear range
4th Gear range
Check your machine tool manual for details.
All rights reserved. Subject to change without notice.
17-April-04
12-1
CNC Programming and Operations Manual
P/N 70000487G - S and M Functions
Miscellaneous Functions (M-Code)
Miscellaneous codes control a variety of machine tool functions. Refer to
Table 12-3. The machine builder assigns them. Be familiar with the
M-codes available on your machine-control combination. M-function
availability varies from one machine to another. Refer to your machine
tool manual for a complete list of M-codes.
Table 12-3, M-Code Controlled Functions
M-Code
M2
M3
M4
M5
M8
M9
M10
M11
M19
M20
M21
Function
Program end
Spindle on forward
Spindle on reverse
Spindle off
Coolant on
Coolant off
U-axis clamp on
U-axis clamp off
Spindle orientation
Disable feed hold
(machine will not feed without spindle on)
Enable feed hold
(machine will feed without spindle on)
Control M-Codes
Control M-codes execute or alter certain CNC functions, such as program
end, subprogram call, mirror image, etc.
These M-codes are part of the CNC software. To use them, write the
appropriate M-code into the program. Refer to Table 12-4.
Table 12-4, Control M-Codes
M-Code
M00
M01
M02
M30
12-2
Function
Program stop. Program stops indefinitely. Press START to
resume.
Optional program stop. If corresponding hardware switch
is ON, M01 acts as M00. If switch is OFF, program will
ignore M01.
NOTE: Appropriate hardware is required for M01.
Program end. At M02, the program stops and returns to
the first program block.
Program end. Return to other program. M30 O75
programmed, as the last block of a main program will return
the CNC to program #75. O75 must be in the same file.
(Continued…)
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - S and M Functions
Table 12-4, Control M-Codes (Continued)
M-Code
M98
M99
M100
M105
M106
M107
M700
M701
Function
Subprogram call. A block in the main program with M98
P100 will execute subprogram 100. O100 must be in the
file after the end of the main program.
Return from subprogram. M99 ends a subprogram and
returns to the main program at the block preceding the last
executed program call.
Mirror image. M100 programmed with axis (M100 X)
activates “mirror image” (ON) for that axis. Mirror image
reverses the sign (+/-) of subsequent numbers. More than
one axis can be mirrored at once (M100 XY). To cancel
mirror image, program M100 on a block by itself.
NOTE: Cutter compensation is mirrored, so switching from
G41 to G42 is unnecessary.
Dry-Run, all axes. Program M105 in a program file or in
MDI to set Dry Run Mode. CNC executes all feed moves at
a rate set by the builder. It enables you to run programs
through quickly to check for mistakes. M107disables DryRun.
NOTE: Making and saving a change to the Setup Utility will
cancel M105.
Dry-Run, NO Z-axis. M106 in a program file or in MDI sets
Dry-Run (No Z) Mode. All feed moves are executed at a
rate set by the builder, and all Z moves are ignored during
the dry-run. This enables you to run through a program
quickly, without Z-axis movement. M107 disables Dry-ZRun.
NOTE: Making and saving a change to the Setup Utility will
cancel M106.
Dry-Run OFF. Cancels M105 or M106. This returns the
CNC to normal operating mode.
Deactivate or set advanced scaling.
Example: M700 X2 Y1.5 will deactivate advanced scaling,
and set the advanced scale factor to 2x for X
and 1.5x for Y.
Activate Advanced scaling. The advanced scaling
function allows the scaling factor to be different for the two
axes (the plane) involved in arcs or circles. In standard
scaling (G72), factors must be the same when cutting arcs.
Only program axes are to be scaled.
Example: M701 XY will activate scaling for X- and Y-axes,
at previously set factors (set by M700).
NOTE: Tool diameter compensation is not allowed with
M700 and M701
(Continued…)
All rights reserved. Subject to change without notice.
17-April-04
12-3
CNC Programming and Operations Manual
P/N 70000487G - S and M Functions
Table 12-4, Control M-Codes (Continued)
M-Code
M800
M801
Function
Deactivate Plane Rotation and Set Angle. You must
program the axis of rotation.
Example: M800 C15 will deactivate plane rotation about
the Z-axis, but set the angle to 15 degrees.
Activate Plane Rotation at Pre-Set Value. (Value set with
M800) You must also program the axis of rotation.
Example: M801 Cxx will activate plane rotation about the
Z-axis at whatever angle was set in C with
M800.
th
Activate 4 (U) synchronization. Axes to be synchronized
must also be programmed.
Example: M900 U will synchronize the U axis with XYZ
feedrate. All moves’ feedrates will be vectored.
6400M
M900
6400M
M901
Deactivate 4th (U) synchronization. Indicate axes to
deactivate synchronization.
Example: M901 U will unsynchronize the U axis with XYZ
feedrate.
M1000
Override Continuous Path parameter. Use M1000 to
override the “Continuous Path” tolerance parameter in the
Setup Utility with a new value. This can be useful if the
CNC hesitates between small moves, such as a 3-D surface
output from CAD-CAM.
Example: M1000 X.125 Y.125 Z .125.
M9244
Servo shut-off code. Typically used if machine is left
unattended for a long period of time. You can place this
code at the end of the program (before M02) to disable the
servos automatically. It is equivalent to pressing E-STOP.
NOTE: ANILAM recommends that you place a G04 T2.0 in
the block before M9244. This enables the servos to
reach definite position before deactivation.
M9351
X302
Clear. Use to clear the Draw Graphics screen at any time.
No other code is allowed on this block.
Order of Execution
The order of execution for available codes is as follows:
T, M, S, F, G, and XYZ (M98 P {sub call} is the exception)
NOTE: Subprogram call (M98 Pn) will always execute last.
12-4
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Communication and DNC
Section 13 - Communication and DNC
Communication
The CNC can exchange data with other RS-232 devices. The baud rate,
parity, data bits, stop bits, and software parameters of the CNC and other
device must agree.
Default communication parameters are entered in the Setup Utility during
machine set up. You can change these parameters from the
Communication screen. Parameter changes made from the
Communication screen are not permanent.
CAUTION: Only qualified personnel should attempt to alter settings
in the Setup Utility. Incorrect settings could disable the
machine.
NOTE: The CNC reloads the setup file at power-on.
Installing the RS-232 Cable
RS-232 communication requires a cable connection between the sending
and receiving machines. Connect the cable to DE-9 connectors on the
CNC chassis and the other machine.
NOTE: The machine builder determines the location of the DE-9
connector.
Use a cable designed for RS-232 communication. On cables designed
for RS-232 Communication, the wires between Pins 2 and 3 are internally
crossed. Data sent from Pin 3 (transmit) of one machine must go to Pin
2 (receive) of the other. Refer to Figure 13-1.
Figure 13-1, RS-232 Communication Connector
NOTE: The same requirements apply for Pins 2 and 3 when one of the
connectors is a DB-25 serial connector.
Computer cables designed as extension cords for computer peripherals
cannot be used for RS-232 Communication because Pins 2 and 3 are not
crossed.
All rights reserved. Subject to change without notice.
17-April-04
13-1
CNC Programming and Operations Manual
P/N 70000487G - Communication and DNC
Accessing the Communication Software
To access the Communication screen:
1. In Manual Mode, press PROGRAM (F2). The Program Directory
activates.
2. Press Utility (F9). The Utility Pop-Up Menu displays.
3. Refer to Figure 13-2. Highlight Communications, and press ENTER.
The Communication screen displays.
NOTE: The default program is highlighted when the Communication
screen is activated.
RS-232 Serial
Communication
Parameters
Program
Figure 13-2, Communication Screen
13-2
PROGRAM
The program selected for
transmission.
SERIAL COMMUNICATION
PARAMETERS
Settings required for the two
machines to send and receive
programs.
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Communication and DNC
Setting Communication Parameters
This manual does not discuss the merits of the different parameter
choices. Refer to an appropriate computer communication guide for
more detailed information.
Selecting the Communication Port
Most CNC installations have at least one RS-232 connector. The
connector is usually mounted somewhere on the cabinet and labeled
RS-232. The CNC is set up to send signals from one of its available
RS-232 ports to the RS-232 connector. This setting cannot be changed.
Personal computers running the off-line software can use COM1 or
COM2 if the hardware supports it.
To select the communication port:
1. In the Communication screen, press Param (F5). The Parameter
Settings menu activates.
2. Select Port. The Settings pop-up menu displays COM1, COM2.
3. Select one.
Setting the Baud
The CNC supports the following bauds: 110, 150, 300, 600, 1200, 2400,
4800, 9600, and 19200.
To set the baud:
1. Select Baud to display the available options. The current setting is
displayed on the Communication screen.
2. In the Communication screen, press Param (F5). The Parameter
Settings menu activates.
3. Select Baud (F2). A pop-up menu displays the available options.
Select one using the arrow keys, F3, F4, and select F5.
4. Set another parameter the same way, or press Exit (F10) to exit to
the previous screen.
Setting Parity
The CNC supports the following parity settings: Odd, Even, and None.
To set the parity:
1. Select Parity to display the available options. The current setting is
displayed on the Communication screen.
2. In the Communication screen, press Param (F5). The Parameter
Settings menu activates.
3. Select Parity (F3). A pop-up menu displays the available options.
Select one.
4. Set another parameter the same way, or press Exit (F10) to exit to
the previous screen.
All rights reserved. Subject to change without notice.
17-April-04
13-3
CNC Programming and Operations Manual
P/N 70000487G - Communication and DNC
Setting Data Bits
The CNC supports the following data bit settings: 7 and 8.
To set the number of data bits:
1. Select Data Bits to cycle through the available options. The current
setting is displayed on the Communication screen.
2. In the Communication screen, press Param (F5). The Parameter
Settings menu activates.
3. Select Data Bits to scroll through the available options. Using Select
(F5), select one.
4. Set another parameter the same way, or press Exit (F10) to exit to
the previous screen.
Setting Stop Bits
The CNC supports the following stop bit settings: 0 and 1.
To set the number of stop bits:
1. Select Stop Bits and press Select (F5) to cycle through the available
options. The current setting is displayed on the Communication
screen.
2. In the Communication screen, press Param (F5). The Parameter
Settings menu activates.
3. Move the cursor to Stop Bits and press Select (F5) to scroll through
the available options. Select one.
4. Set another parameter the same way, or press Exit (F10) to exit to
the previous screen.
Software Setting
The CNC supports the following protocol settings: On and OFF.
Software protocol is frequently referred to as “Xon” or “Xoff”. In
commercial communication packages, this is known as “handshaking”
To set the protocol:
1. Select Software to cycle through the available options. The current
setting is displayed on the Communication screen.
2. In the Communication screen, press Param (F5). The Parameters
Settings menu activates.
3. Move the cursor to Software and press Select (F5) to scroll through
the available options. Select one.
4. Set another parameter the same way, or press Exit (F10) to exit to
the previous screen.
13-4
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Communication and DNC
Setting Data Type
The CNC supports the following data display types: ASCII and Binary.
This setting does not affect the data exchanged; only how it is displayed
on the screen during transmission.
To set data type:
1. Select DataType to cycle through the available options. The current
setting is displayed on the Communication screen.
2. From the Communication screen, press Param (F5). The
Parameters Settings menu activates.
3. Move the cursor to DataType and press Select (F5) to toggle
between the two options. Select one.
4. Set another parameter the same way, or press Exit (F10) to exit to
the previous screen.
Testing the Data Link
The CNC has a utility with which to test the data link. For testing, the
CNC must be connected to another machine. Set the parameters on
both machines. If the other machine has a manual test screen, activate
it.
All rights reserved. Subject to change without notice.
17-April-04
13-5
CNC Programming and Operations Manual
P/N 70000487G - Communication and DNC
Activating the Test Link Screen
With the Communication screen active, press TestLnk (F8). The Test
Link screen activates. Refer to Figure 13-3.
Figure 13-3, Test Link Screen
Setting Test Link Display Modes
To test the link, visually verify that the test data sent matches the test
data received. The Data type setting determines how characters appear
on the screen.
If Data type is set to ASCII, letters and numbers are displayed. If the
data type is set to Binary, the hexadecimal equivalent is displayed. Set
both machines to use the same data display type.
NOTE: Hexadecimal characters appear as pairs of numbers or numbers
and letters.
To change the Link Test screen data display:
1. From the Link Test screen, press Param (F9) to switch between
ASCII and Binary Modes. The current mode is displayed in the
settings area of the Link Test screen.
13-6
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Communication and DNC
Testing the Link
1. Set up an RS-232 connection with another machine (or computer).
2. Set the other machine to receive.
3. With the Link Test screen active, use the CNC’s keypad to enter any
series of numbers. This data will appear in the transmit area.
4. Verify that the other machine has received the data correctly.
5. Set the other machine to transmit.
6. Manually transmit data from the other machine.
7. Verify the CNC receives the data in the Receive Area. The test is
complete.
Clearing the Receive Area
Press ClearRx (F3) to clear the Receive Area.
Clearing the Transmit Area
Press ClearTx (F5) to clear the Transmit Area.
Sending a Program
The name of the program highlighted when the Communication screen
was activated is listed next to the PROGRAM label on the screen. The
CNC sends this program unless you select another program. The CNC
prompts to select another program during the sending process.
1. With the Communication screen active, the parameters set and the
link tested, press Send (F3). The CNC prompts to send the selected
program or to change the program being sent.
2. Press Select (F1). The CNC sends the program.
– or –
Press Other (F3). Enter the name of the desired program.
Receiving a Program
You must enter a name for received programs before you receive them
from the other machine.
To receive a program:
1. With the Communication screen active, the parameters set and the
link tested, press Receive (F1). The CNC prompts to enter a name
for the incoming program.
2. Type the desired name, and press ENTER. The CNC displays a
READY TO RECEIVE . . . message.
3. Start transmitting from the sending machine.
All rights reserved. Subject to change without notice.
17-April-04
13-7
CNC Programming and Operations Manual
P/N 70000487G - Communication and DNC
Setting the Transmission and Receiving Display
If the CNC is transmitting or receiving with the Text Mode active, the
exchanged program will be displayed on the screen. If the Text Mode is
off, the display area will remain blank.
Text (F6) is highlighted when the Text Mode is active.
The “Transfer In Progress” symbol (just above the soft key line) cycles
when data is exchanged.
Press Text (F6) while transmitting or receiving to switch the CNC in and
out of Text Mode.
Holding Transmission/Receiving Operations
When sending or receiving programs the operation can be paused by
Press Hold (F1) to pause an operation while sending or receiving
programs. Press Resume (F2) to continue the exchange.
NOTE: If the CNC is receiving a program and either machine’s software
parameter (Xon/Xoff) is set to OFF, there is a possibility a hold
will overload the CNC’s buffer, causing portions of the program
to be lost. ANILAM recommends that you operate with the
software parameter (Xon/Xoff) set to ON.
Using Data Control (DC) Codes
Data Control (DC) codes are sometimes required to automate the
operation of a paper tape reader or punch.
Refer to Table 13-1 for the available DC Codes. The ASCII column lists
the codes required to perform the corresponding “Function.” The Hex
Code is the hexadecimal equivalent of the ASCII code. The CNC Key
column lists the key you press on the CNC keypad or a PC keyboard to
transmit the required DC code.
Table 13-1, DC Codes
ASCII
DC1
DC2
DC3
DC4
Function
Reader Start
Punch Start
Reader Stop
Punch Stop
Hex Code
CNC Key
0x11
0x12
0x13
0x14
1
2
3
4
A reader or punch will turn ON (start) or OFF (stop) in response to these
codes. To test reader or punch communication, activate the
Communication screen and press any of these keys. The paper tape
reader or punch should respond appropriately.
13-8
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Communication and DNC
Using DC Codes In Receive Mode
Usually a receive operation involves the paper tape reader. You must
start the reader, thereby initiating the reading of the paper tape. Do this
after the CNC has been set up to receive the file.
1. Set up to the CNC to receive a program.
2. Press 1 to send the DC1 code to the reader. The reader starts.
3. After the CNC has read the tape, press 3 to stop the reader, if
necessary. The CNC sends the DC3 code to the reader and the
reader stops.
Using DC Codes In Send Mode
Usually, a send operation involves the paper tape punch. Set up and
start the punch prior to initiating the send operation.
1. Select the program that will be sent to the tape punch.
2. Press 2 to send the DC2 code to the punch. The punch starts.
3. Press Send (F3) to start sending the program. If necessary, change
the name of the program.
4. When the program has been completely transferred to the punched
tape, press 4 to stop the punch, if necessary. The CNC sends the
DC4 code to the punch and the punch stops.Running in DNC
Direct Numeric Control (DNC) is also known as Continuous Downloading.
This function is used only when it is necessary to run a program that is
larger than the CNC’s available memory.
NOTE:
Before you use the DNC function, ensure that all setup
procedures are completed. Set Part Zero and make necessary
Tool Page Entries.
NOTE: To quit the DNC function after it has started, press DNC (F4)
then press Exit (F10) twice. The CNC will revert to Manual
Mode.
The DNC screen is similar to other operating screens, but with
communication information added. Refer to Figure 13-4, DNC Screen.
All rights reserved. Subject to change without notice.
17-April-04
13-9
CNC Programming and Operations Manual
P/N 70000487G - Communication and DNC
Accessing DNC
1. In the Program screen, press Utility (F9). A pop-up menu displays.
2. Highlight Communications, and press ENTER. The Serial
Communication Parameters screen displays.
3. Press DNC (F4). Press Receive (F1). The CNC is now ready to
begin receiving a program from an offline (host) computer.
Once the transmission is started from the offline machine, the CNC
performs as usual. Tool changes, Single-Step Mode and Real Time
Draw function as described in other sections.
Figure 13-4, DNC Screen
Total Blks Rec:
The total number of program blocks the
CNC has received at that point.
% Receiving Buffer Full
Percentage of receiving buffer used.
% Executing Buffer Full
Percentage of executing buffer used.
Via RS-232, programs are transmitted faster than they can be executed.
This makes it necessary to manage the memory and timing between the
two machines.
The CNC uses two buffers. One buffer receives the incoming program
while the contents of the second buffer is executed. When the executing
buffer is empty, they swap. The CNC executes the contents of the full
buffer while the empty buffer receives additional data.
When the software protocol (Xon/Xoff) is used, the CNC can signal the
sending machine to pause until it has a buffer with room to receive.
13-10
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Communication and DNC
NOTE: Most machines default to the buffer mode for DNC operations.
Some machines may be set to default to the Drip Feed Mode for
DNC. In Drip Feed Mode, program blocks are transmitted and
executed one at a time, without buffering.
To put the CNC in Direct Numeric Control Mode:
1. With the Communication screen active, parameters set and the link
tested, press DNC (F4). The DNC soft key labels appear.
2. Press Receive (F1). The DNC screen activates and the message line
prompts to begin transmitting from the other machine. Once the
receive buffer is full, the CNC prompts to press START.
3. Press START. The CNC runs the incoming program.
All rights reserved. Subject to change without notice.
17-April-04
13-11
CNC Programming and Operations Manual
P/N 70000487G - Machine Software and Peripherals Installation
Section 14 - Machine Software and Peripherals Installation
Machine Software Installation
The CNC software is installed when the machine is set up and during
software updates.
To install the machine software:
1. In Manual Mode, press [SHIFT + EXIT (F10)]. The CNC's startup
screen displays.
2. Highlight Setup Utility, and press ENTER. The Setup Menu displays.
3. Highlight Software Update, and press ENTER. The installation
sequence begins.
4. Follow the instructions on the screen.
Keyboard Installation (Option)
The machine builder determines whether the system will support a
keyboard option. If the system supports a keyboard, plug the keyboard
DIN connector into the computer chassis.
WARNING:
There is no keyboard equivalent for the E-STOP.
Therefore, emergency shutdowns (E-STOP) cannot be
performed via keyboard.
NOTE: Industrial grade keyboards are recommended for shop
environments.
All rights reserved. Subject to change without notice.
17-April-04
14-1
CNC Programming and Operations Manual
P/N 70000487G - Machine Software and Peripherals Installation
Keypad Equivalent Keyboard Keys
Refer to Table 14-1.
Table 14-1, Keyboard Equivalents
Function
CNC Key Face
CLEAR
(ALT + C)
– or –
DELETE
ARROWS
ARROWS
ENTER
ENTER
X (axis)
(X)
Y (axis)
(Y)
Z (axis)
(Z)
U (axis)
(U)
START
(ALT + S)
HOLD
(ALT+ H)
Activate System Refer to “Displaying
Information
System Information” in
Screen
“Section 10 - Program
Management.”
14-2
Keyboard Keystroke
Equivalent
(ALT+ I)
Activate
Enlarged
Position Display
(B)
Switch to Rapid
Override
(R + ENTER)
Activate PLC
Monitor
(P)
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Off-line Software Installation
Section 15 - Off-line Software
The off-line version of the software requires an **Intel® based Personal
Computer (PC) or 100% compatible. A minimum of 4MB of RAM is
required. The hard disk drive must have a minimum of 4MB of space
available.
The off-line software is also compatible with **Microsoft® **Windows®
Operating Systems, such as **Windows NT®, Windows 95, Windows 98,
or Windows 2000.
Passwords
Access to some parameters is restricted. Refer to Table 15-1. When
required, the CNC prompts you to enter a password.
To access protected parameters:
1. Type the service password, and press ENTER. The CNC allows you to
change the protected settings.
2. Passwords protect four access levels. Operators are assigned limited
passwords, which enable them to set parameters used in normal
machine operations. Service passwords enable a higher level of
access. The factory password is not used outside the manufacturer’s
plant.
Table 15-1, Off-line Passwords
Restriction Level
Limited access
Service access
Integrated Programmable Intelligence (IPI)
Password
Q1
Q2
Q3
Exiting the Software
Press ESC to exit the software from the Main Menu selection screen.
-----
**
**
Intel® is a registered trademark of Intel Corporation in the United States and/or other
countries.
Microsoft®, Windows®, and Windows NT® are registered trademarks of Microsoft
Corporation in the United States and/or other countries.
All rights reserved. Subject to change without notice.
17-April-04
15-1
CNC Programming and Operations Manual
P/N 70000487G - Off-line Software Installation
Windows Off-line Software Installation
1. Insert the installation disk in the floppy drive.
2. Go to the task bar and click on the Start button. Select Run. The
Run window activates.
3. In the Open entry field, type A:setup. Click on OK. The installation
procedure will begin.
4. Follow the on-screen prompts as they appear.
NOTE: Substitute B:setup for A:setup if your 3.5 inch floppy is in
the B:-drive.
Running Off-line Software from Windows
1. If you selected Desktop Icon (recommended) during the installation,
click the CNC icon on your desktop.
2. If you selected Start Menu, start from there.
System Settings
Maximum Memory Allocated
In the Setup Utility, you can adjust the amount of memory allocated to the
CNC software. Set the Maximum Memory Allocated parameter
between 2 MB and 18 MB. This feature limits the amount of memory
available to the software, preventing the CNC program from tapping into
Windows’ large virtual memory supply. Allocating too much memory to
the control software will dramatically increase startup time and make the
software run slower.
To change the Maximum Memory Allocated, do the following:
1. In the CNC startup screen, select Setup Utility, and press ENTER.
The Setup Options menu displays.
2. Select Machine Constants, and press ENTER. The Machine
Constants menu displays.
3. Select MC_1014: Maximum memory allocated, and press ENTER.
Type the appropriate value, and press ENTER.
The only time it might be necessary to increase this parameter is when
editing a program that is larger than this value. In this case the CNC will
generate an error message indicating that there is not enough memory to
edit the program. To correct this problem, change this parameter to the
size of program plus 1MB.
15-2
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Off-line Software Installation
Disabled Features
The following software features, found in the Program Directory’s Utility
(F9) pop-up are not available under any Windows operating system:
Check Disk
q Floppy Format
q Disk Optimization
q Program Restore
If you select one of these features, the CNC displays a message that the
feature is disabled.
q
All rights reserved. Subject to change without notice.
17-April-04
15-3
CNC Programming and Operations Manual
P/N 70000487G - Four-Axis Programming
Section 16 - Four-Axis Programming
Axis Types
6400M
6000M-4X
The machine builder sets up the fourth-axis as linear, rotary or readout
axes. The three basic axes are X, Y, and Z. The additional axis is
designated as U (6000M-4X). This section will discuss the rotary axis
option in detail.
Below are the programming formats for linear or rotary additional axes:
Linear:
Program as Feed Mode (G1) or Rapid (G0) moves. Only
rapid and linear feed moves can be programmed. You must
set an individual feedrate if a move is non-synchronous
(Format: FU 20.0). U can be programmed along with X, Y,
and Z-axis in rapid, linear, and circular moves. You can make
U synchronous or non-synchronous to the XYZ moves.
Program Sync codes:
M900 U
(for synchronous)
M901 U
(for non-synchronous)
on a block alone. No other code is allowed on the sync block.
Rotary:
Program rotary moves in degrees. The typical resolution is
0.001 degrees (set by builder). Minutes and seconds cannot
be programmed. Therefore, you must convert minutes and
seconds to a decimal value.
Conversion formula for minutes, seconds to decimal degrees:
Minutes to decimal: min/60 = decimal degrees.
Example: 15 min/60 = 0.25 degrees
Seconds to decimal: sec/3600 = decimal degrees
Example: 30 sec/3600 = 0.008 degrees
Example:
5 deg. 30 min. 15 sec. =
5 + (30/60) + (15/3600) =
5 + 0.5 + 0.004 =
5.504 degrees
You must program feedrates for non-synchronous moves. Program the
feedrate in degrees per minute (dpm).
Format:
FU 500.0 = 500 dpm for the U axis.
All rights reserved. Subject to change without notice.
17-April-04
16-1
CNC Programming and Operations Manual
P/N 70000487G - Four-Axis Programming
Rotary Axis Programming Conventions
A rotary axis (typically U) will program differently based on the setting of
the Reset Rotary at 360 parameter, which is determined by the builder.
The default for this parameter is No; in which case, the U-axis behaves
like a linear axis. If set to Yes, the behavior of the rotary axis (U) is
described below.
If programming the U-axis in Absolute:
The rotary axis will never rotate more than 180 degrees in one move. So,
if a move of greater than 180 degrees is programmed, the control will
resolve the number to a positive value less than 360 degrees and move
to that target, taking the shortest distance (always less than 180
degrees). A move of exactly 180 degrees will always move positive and
a move of exactly 360 degrees will not move at all.
If programming the U-axis in Incremental:
The rotary axis will move the exact amount of degrees programmed and
in the direction indicated with the plus or minus sign. The display will
reset to zero every time 360 degrees is crossed so that the highest value
in the U-axis display will be 359.999 degrees depending on the displayed
resolution.
Non-Synchronous or Synchronous Auxiliary Axis
You must decide whether the fourth-axis move will be synchronous or
non-synchronous. A synchronous move is defined as a move in which all
axes programmed (XYZU) reach target simultaneously. Use
synchronous moves to thread-mill along a rotary axis or to machine an
impeller part. Usually, the programmer uses an M-Code to set
synchronization ON (Sync-On) or OFF (Sync-Off) for the designated
axes. [Default: Sync-Off]
Format: M900 U
Example: N110 M900 U sets Sync-On for U-axis only. If a U dimension
is programmed on the same block as any rapid, linear feed, or circular
XYZ move, the U axis will reach target simultaneously with the other
axes. The feedrate (Fn) programmed for the XYZ move (X, Y, Z, XY, XZ,
YZ, or XYZ) will be applied along the vector of the cut. If you program 10
IPM (F10), the CNC adjusts the feedrates along each axis so that tool
movement equals 10 IPM (vector speed). The feedrate displayed on the
CNC screen is the vector feedrate.
Synchronous moves are used only when necessary. For example, you
want to thread mill a part, with the centerline of the rotary axis parallel to
the X-axis. Synchronize X and U. Turn sync OFF when not in use.
16-2
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Four-Axis Programming
Format: M901 U
Example: N110 M901 U will set Sync-Off for U axis only. If a U
dimension is programmed on the same block as any rapid, linear feed, or
circular XYZ move, the U axis will not reach target simultaneously with
the other axes. The feedrate (Fn) programmed for the XYZ move (X, Y,
Z, XY, XZ, YZ, or XYZ) will be applied along the vector of the cut. A
separate feedrate is programmed for U (FUn). The feedrate
programmed for XYZ (Fn) will be applied to those axes.
Generally, Nonsynchronous moves are used for indexing work such as
milling a side of a part or drilling at various rotary locations.
NOTE: Sync-ON and Sync-OFF is set individually. M900 U sets U ON.
M901 U sets U OFF.
Nonsync fourth-axes moves require a separate feedrate for the additional
axes (FUn). If you do not program a separate feedrate, the U feedrate
will be based on the vectored feedrate of Fn.
Feedrate display is either XYZ (Sync-Off) or vectored (Sync-On).
In a 4-axis setup, the rotary table is set so the centerline of the rotary axis
is parallel to the X-axis. If the U-axis is linear, the same M-Codes apply.
4-axis setups are often a combination rotary/tilt table mounted setup.
The rotary range is +/- 360 degrees, and the tilt range is 0 to 90 (flat to
vertical).
If programmed with Ellipse (G05) or Spiral (G06), the fourth axis must be
positioned in the block after the XYZ coordinates and before the IJK
coordinates.
Programming Examples
All programming examples are for 4-axis machining with the rotary table
mounted on the left end of the mill table, with the centerline of the rotary
axis parallel to the X-axis. The face of the rotary table faces X+.
The examples contain both milling and drilling applications. Modal cycles
G81 to G89 and G66 can be executed at rotary locations as in XYZ
locations. Non-modal canned cycles can be executed at rotary locations.
Use sync-OFF and position the rotary axis before you execute the cycle.
All rights reserved. Subject to change without notice.
17-April-04
16-3
CNC Programming and Operations Manual
P/N 70000487G - Four-Axis Programming
Example 1: Drill (Sync-Off)
Mount the fourth axis as described above. Mount a part 6-inches wide
and 8-inches long on the face of the rotary table. Reset Rotary at 360 is
set to No.
Table 16-1 shows a drilling example with No Sync. You must drill ten
0.375-inch holes 36-degrees apart, 1-inch deep, 0.75-inches in from the
end of the cylinder. Then, starting at X-2 U0, drill a spiral series of holes
36-degrees and X-0.500 inches apart each. Set X0 at the right end, Y0
at the cylinder's centerline, U0 at a pre-milled keyway on the cylinder.
Measure tool offsets from the top of the cylinder, with Y-axis at 0.
Table 16-1, Four-Axis Example 1
* 4-AX-DRL
* SET RESET ROTARY AT 360 TO "NO"
G90 G70 G0 T0 Z0 U0 M5
X0 Y0
T1 *#3 CENTERDRILL
M3 S2400
G81 Z-.22 R.1 F12
M98 P1
T2 * 3/8" DRILL
M3 S1850
G87 Z-1 R.1 F14 I.18 J.012 K.1 U.3334
M98 P1
M2
O1 * ROTARY HOLE LOCATIONS
G0 G90 X-.75 Y0 U0
LOOP 9
G0 G91 U36
END
G0 G90 X-2 U0
LOOP 9
G0 G91 X-.5 U-36
END
G80
M5
G0 G90 Z0 T0
X0 Y0 U0
M99
16-4
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Four-Axis Programming
Example 2: Mill (Sync-On)
Mount the fourth axis as described above. Mount a part 3 inches in
diameter and 5 inches long on the face of the rotary table. The part has
a 0.25-inch radius turned on the end. Reset Rotary at 360 is set to No.
Table 16-2 shows a milling example only. Assume that a series of six
0.25-inch wide grooves must be milled 60-degrees apart, 0.25-inch deep at
the start, tapering up to 0.125-inch deep and rotating 15 degrees at the far
end. The groove must follow the end contour of the part (radius). Set X0
at the right end, Y0 at the cylinder centerline, U0 at a pre-milled keyway on
the cylinder. Set the tool offset so that the centerline of the 0.25-inch ballend mill is at the centerline of the 3-inch diameter part (with Y axis at 0).
Table 16-2, Four-Axis Example 2
* 4-AX-MILL
* SET RESET ROTARY AT 360 TO "NO"
G90 G70 G0 T0 Z0 U0 M5
X0 Y0
T1 *.25 BALL-END-MILL
S2400
M3
M98 P1 L6
G90 G0 T0 Z0 M5
G0 X0 Y0 U0
M2
O1 * GROOVE
G90 G0 X.225
G0 Z2.625
G1 X.125 F5
M900 U
G18 G91 G2 X-.25 Z.25 I-.25 K0 U-2.
G17 G1 X-3.25 Z.125 U-13
M901 U
G90 G0 Z3.225
G0 X.225
G91 G0 U-45
M99
All rights reserved. Subject to change without notice.
17-April-04
16-5
CNC Programming and Operations Manual
P/N 70000487G - Four-Axis Programming
Example 3: Mill (Sync-On)
Mount a fourth axis as described above. Mount a part 4-inches in
diameter and 8-inches long on the face of the rotary table. Support the
part on the X+ end by a live center. The part has a 0.25-inch, 45-degree
chamfer on one end. Reset Rotary at 360 is set to Yes. This will
prevent the need to unwind the U-axis, saving operation time.
Table 16-3 shows a thread-milling example. Assume that a 4-8 UN 2A
thread must be milled from the right end, 6-inches long. The tool is
tapered to conform to the thread. Set X0 at the right end, Y0 at the
cylinder's centerline, U0 at a pre-milled keyway on the cylinder. Measure
the tool offset from the top of the part (with Y axis at 0).
The X start position will be one pitch (0.125 in.) to the right of X0, so that
the tool enters the work smoothly.
Table 16-3, Four-Axis Example 3
* 4-AX-THD
* SET RESET ROTARY AT 360 TO "YES"
G90 G70 G0 T0 Z0 U0 M5
X0 Y0
T1 * SPECIAL THD-TOOL
S3500
M3
G0 X.125 Y0 U0
Z.1
G1 Z-.075 F80
M900 U
* SET RESET ROTARY AT 360 TO "YES"
* THIS IS TO PREVENT THE NEED TO UNWIND U
* U AXIS MOVE IS
* (360 X 8 PITCH X 6" LONG)
* + 360 FOR 1 TURN X.125 LEAD-IN
* U MOVE WILL BE 17,640.00 DEGREES
* OR 49 TURNS
G91 G1 X-6.125 U((360*8*6)+360)
M901 U
G90 G0 T0 Z0 M5
X0 Y0 U0
M2
16-6
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - DXF Converter Feature
Section 17 - DXF Converter Feature
The DXF Converter feature allows information in a Drawing Exchange
File (.DXF extension) to be used to create a CNC conversational
(.M extension) or G-code (.G extension) file.
Contours and drill hole locations in the DXF file can be put in the CNC file
in the form of subroutines, using a mouse and “point and click” approach.
The DXF Converter feature creates a CNC program that must be edited
to be usable, but most of the program creation is already done.
Requirements
Off-line Software
The Personal Computer (PC) must have a mouse installed. The Anilam
Off-line Software is required. The Anilam Off-line Software will run in an
MS-DOS or Windows environment. (See “Section 15 - Off-line
Software.”)
Machine Software
A mouse or other pointing device (for example, track ball) must be
installed to properly operate the DXF converter on the machine. As part
of installing a mouse, it is necessary to install a driver. A suitable driver
should be included with the mouse when purchased. Follow the
manufacturer's instruction to install an MS-DOS compatible driver.
Typically, this will require editing AUTOEXEC.BAT and adding a line to
load the mouse driver before the CNC software starts running. See
sample AUTOEXEC.BAT below. The mouse can be a serial mouse or a
PS/2 style mouse (PS/2 style mouse only supported on systems
manufactured after January 1, 2003). The serial mouse must be
connected to the RS-232 port. If using a PS/2 style mouse, it must be
connected to the keyboard connector on the console through a PS/2
Y-splitter cable. The mouse will only be operational while in the DXF
Converter. Depending on the mouse and mouse driver, it may be
necessary to have the mouse connected before turning the CNC on.
ECHO OFF
PROMPT $P$G
PATH C:\;C:\DOS
ECHO Loading CNC software
SET P5MSYS=C:\P5M
C:
CD \P5M
\MSMOUSE\MOUSE
<<<< Line added to load mouse driver
P5M
All rights reserved. Subject to change without notice.
17-April-04
17-1
CNC Programming and Operations Manual
P/N 70000487G - DXF Converter Feature
Entry to the DXF Converter
To open the DXF Converter:
1. Open the Anilam Off-line Software
2. Gain access to the Program page and highlight the DXF file you wish
to convert. For details on how to work with the Program page see
“Section 10 - Program Management.”
3. Select the Utility soft key to display a pop-up menu
4. Select DXF Converter on the pop-up menu to bring the drawing into
the DXF Converter.
The drawing display screen shows the file name in the upper-left border,
the current X Y position of the mouse pointer at the upper-right corner, a
message and information area along the bottom border, and several soft
keys along the bottom edge.
Creating Shapes
The part drawing is used to create shapes. Shapes are then output to
CNC programs as subroutines. There are many features to make the
drawing screen easier to use. Layers may be turned on or off. Any area
of the screen can be zoomed in or out. Refer to Table 17-1, Mouse
Operations and Table 17-2, DXF Hot Keys.
Each shape is given a sequential number. The number is displayed on
the screen at the beginning of the shape. Press F1 to toggle Select mode
on. With Select mode on, entities can be selected to be part of a shape.
Left click with the mouse to make selections. When an entity is selected,
it will change color.
When selecting entities, direction is determined by where the mouse
pointer is positioned. If nearer the left side of a line, direction will be left
to right.
There are two types of shapes:
q
q
17-2
One used for contouring or feed motion
One for drilling a series of holes
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - DXF Converter Feature
Contours
Pick an entity where the shape will begin. Pick the last entity in the
shape. All entities that are connected will be chained together and
change color to verify this. Some shapes have to be selected one entity
at a time. This is determined by the way the part was drawn in the DXF
file.
If an entity is selected that is not connected to the previous one, a
message is displayed, “Entity not connected, connect anyway (Y/N)?”
Answering Yes will join and allow the shape to be continued. This is
sometimes needed when the drawing was not properly made. The same
message is displayed when a shape is finished and a new shape is
started. Answering No produces a second message, “Create new shape
(Y/N)?” If this is answered Yes, a new shape number is displayed.
Entities in a shape can be un-selected by clicking them again. This
un-selects everything previously selected to that point. To delete a
shape, click on the first entity.
Drilling
When circle entities are selected, they are assumed to be drilling hole
locations. As circles are selected, a dotted line shows the rapid path
between holes. Selecting anything other than a circle, ends the drilling
shape and produces the message, “Create new shape (Y/N)?”
If you wish to create a second drilling shape, select the first hole of the
next shape by right clicking the mouse. The message, “Create new
shape (Y/N)?” is displayed.
CNC Code
Each shape that is created is made into a subroutine. If the option was
selected as a setup parameter, for each subroutine, there is a call in the
main program. (Refer to Table 17-4, Output Menu Descriptions.)
Running the CNC program in Draw mode allows the tool paths to be
seen.
The file must be edited to add tool numbers, feed rates, cutter comp on or
off, and so forth.
The tool paths are only as accurate as the DXF drawing file used.
The Output Parameter pop-up menu contains a Shift X and Shift Y entry.
The purpose of these entries is to shift the X Y coordinate system of the
CNC program. This is usually done, since the coordinates in the drawing
file are based from some corner of the drawing and it is preferable to use
some feature of the part as the X0 Y0 position. Refer to “Shift X, Shift Y
Descriptions” later in this section.
All rights reserved. Subject to change without notice.
17-April-04
17-3
CNC Programming and Operations Manual
P/N 70000487G - DXF Converter Feature
Additionally, each DXF shape can be saved as a CAM Shape for use in
the CNC's CAM utility. If the Output format parameter (Refer to
Table 17-4, Output Menu Descriptions) is set to CAM Shape, the DXF
shapes are saved as CAM shape files. One CAM shape file is created for
each DXF shape being saved. Any existing shape file is overwritten.
These files can then be imported into a CAM program by using the
Recover Shapes feature under Misc in CAM. Complete CNC code can
then be generated using the imported shapes and the Motion features in
the CAM utility.
Mouse Operations
Refer to Table 17-1 and Table 17-2, DXF Hot Keys.
Table 17-1, Mouse Operations
17-4
Button
Event
Function
Left
Press–Drag–Release
Zoom Window
Right
Press–Drag-Release
Pan
Left
Double click
Zoom Fit
Left
Click Top Edge
View XY Plane
Left
Click Right Edge
View YZ Plane
Left
Click Bottom Edge
View XZ Plane
Left
Click Left Edge
View ISO
Left
SHIFT +
Click
Zoom In
Right
SHIFT +
Click
Zoom Out
Left
Click (Select mode on)
Select Entity
Right
Click (Select mode on)
Link Unconnected Entities or
Create New Shape
Left
CTRL
+ Click
Basic Entity Information is
displayed on the bottom of
the screen.
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - DXF Converter Feature
DXF Hot Keys
Refer to Table 17-2.
Table 17-2, DXF Hot Keys
Hot Key
Event
Hot Key
Event
ALT + A
Zoom Fit
ALT + N
All Layers On
ALT + B
Redo View Change
ALT + O
View Plane ISO
ALT + C
Erase Text
ALT + P
Toggle Axes
ALT + D
Zoom In
ALT + Q
Quit / Exit
ALT + E
Set Chain Delta
ALT + R
Redraw
ALT + F
Toggle Entity Endpoints
ALT + S
Save Shape to Output Filename
ALT + G
Toggle Dotted Grid
ALT + T
Paste Entity Info to Shift Field
ALT + H
Zoom Out
ALT + U
Undo View Change
ALT + K
Cycle Tracking Resolution
ALT + X
View Plane XY
ALT + L
Toggle Layers
ALT + Y
View Plane YZ
ALT + M
Invert Layers
ALT + Z
View Plane XZ
Toggle Entity Endpoints (ALT + F)
This hot key places a small X at the end of every entity. If a shape is not
chaining as expected, using this feature helps determine the problem.
Look for X’s in unexpected positions. Two lines may be overlapped, for
example.
Using the mouse (CTRL + left click) with endpoints on will ‘flash’ each
entity and also provide more information. Zoom the problem area for the
best view.
All rights reserved. Subject to change without notice.
17-April-04
17-5
CNC Programming and Operations Manual
P/N 70000487G - DXF Converter Feature
DXF Soft Keys
Refer to Table 17-3.
Table 17-3, Soft Key Descriptions
Soft Key
Function
Description
F1
Toggle Select Mode
Select mode must be on when chaining
shapes.
F3
Layers Menu
Pop-up menu has:
§
§
§
All Layers on
Invert Layers
Toggle Layers
Layers can be turned on or off as desired.
NOTE: The mouse (CTRL + left click), that is
hold down the CTRL key while left clicking an
entity, provides the layer name of the clicked
entity at the end of the basic entity information
displayed at the bottom of the screen. This is
helpful to determine which layers to turn on
and/or off.
F4
View Menu
Pop-up menu has: XY, XZ, YZ, and ISO
selections.
F5
Display Menu
Pop-up menu has: Fit, Window, Redraw, Half,
and Double. Select the desired display.
F6
Misc.
Pop-up menu has: Entity Info, Set Shift,
Toggle Endpoints, and Link or New Shape.
Select the desired option. See “Miscellaneous
DXF Soft Key, F6” for details.
F8
Save
Creates CNC code. The message,
“Successfully created (filename) (.M or .G).” is
displayed when Save is activated. If no
shapes are defined, a warning message is
displayed.
F9
Setup
Pop-up menu provides access to Output or
Display parameters. Refer to Table 17-4,
Output Menu Descriptions and to
Table 17-5, Display Menu Descriptions.
(Continued…)
17-6
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - DXF Converter Feature
Table 17-3, Soft Key Descriptions (Continued)
Soft Key
Function
Description
F10
Exit
F10 exits the Setup menus, exits the DXF
Converter, and returns to the Program page.
Be sure to Save (F8) any work done before
exiting. Anything not saved will be lost.
If shapes have been created, a message, “Exit
(Y/N)?” is displayed. This is a reminder to be
sure you have saved your work.
Miscellaneous DXF Soft Key, F6
Press Misc. (F6) to display the miscellaneous DXF pop-up menu with the
following options:
Entity Info
Displays entity information at the bottom of the
screen. (See Table 17-1, Mouse Operations.
This option is equivalent to pressing
(CTRL + left click).
On the off-line or using an auxiliary keyboard,
the Entity Info is displayed by holding the CTRL
key when you pick the entity.
Set Shift
Pastes the Entity Info onto the Shift field.
(See Table 17-2, DXF Hot Keys. This option
is equivalent to pressing (ALT + T).
Toggle Endpoints
Toggles entity endpoints.
(See Table 17-2, DXF Hot Keys. This option
is equivalent to pressing (ALT + F).
Link or New Shape
When creating a shape, select this option to
terminate the current shape or to add new
entities to the current shape. When a new
entity is selected, the “Connect to existing
shape (Y/N)?” message is displayed. To
continue, press Yes (F1) or No (F2).
All rights reserved. Subject to change without notice.
17-April-04
17-7
CNC Programming and Operations Manual
P/N 70000487G - DXF Converter Feature
Output Menu Options
Refer to Table 17-4.
Table 17-4, Output Menu Descriptions
Parameter
Default
Input Definition
Output program name
DXF filename
Different filename. No extension required.
Shift X
0.000
X position offset value
(See “Shift X, Shift Y Descriptions.”)
Shift Y
0.000
Y position offset value
(See “Shift X, Shift Y Descriptions.”)
Output dim.
Absolute
Incremental or Absolute.
Create mode
Smart
Overwrite or Smart.
Overwrite replaces existing program file.
Smart replaces duplicate subs only.
Starting sub number
1
Beginning sub number. To keep previously
created subs, use next higher number.
Output format
G-code
G-code/ISO, Conversational, or CAM Shape
Output warnings
Yes
Yes or No. A setting of Yes outputs warnings
in the program.
Re-calc Intersections
Yes
Yes or No. A setting of Yes re-calculates the
intersections in the DXF file.
Output resolution
5
Number of decimal digits ( 3 to 6 )
Create main in new
Yes
Yes or No
No will not create main to call subs in new
programs.
Convert values
None
None or (to)Metric or (to)Inch
Convert polyline
None
None, To Arc, or Prompt
(See “Convert Polyline Descriptions.”)
Shift X, Shift Y Descriptions
The end of an entity or center of a circle can be used to automatically
make this point the X0 Y0 of the program. To select the desired point:
1. Use the mouse (CTRL + left click) to display Basic entity information.
2. Press (ALT + T) to paste the coordinates into the Shift XY fields.
A line or arc entity uses the end closest to the mouse pointer.
17-8
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - DXF Converter Feature
Convert Polyline Description
Some DXF files have arcs as polylines. Set the parameter Convert to
Arc to Yes to have an arc output in the CNC program.
Polylines that are not converted to arcs are executed as a series of short
line moves.
Circles that have been converted to polylines by the DXF file creation
software cannot be used for hole drilling or circle center information.
Hence, given the option, it is the best choice that arcs and circles not be
converted to polylines when creating the DXF file.
Display Menu Options
Refer to Table 17-5.
Table 17-5, Display Menu Descriptions
Parameter
Default
Input Definition
Mouse position
resolution
4
Number of places to display
Axes
Off
Toggle display of axes
Grid
None
None, Solid, Dotted
Grid size
1
In current units
Chaining accuracy
.0001
Maximum separation between chainable entities
Picking accuracy
3
Pixel distance from pointer to selected entity
Shape color
Green
Choose color
Entity flash color
Yellow
Choose color
All rights reserved. Subject to change without notice.
17-April-04
17-9
CNC Programming and Operations Manual
P/N 70000487G - DXF Converter Feature
DXF Entities Supported
See Table 17-6 for the DXF entities supported.
Drawing
Transformation
Chaining
Information
Table 17-6, DXF Entities Supported
Line
X
X
X
X
Point
X
X
Circle
X
X
X
X
Arc
X
X
X
X
Trace
X
X
X
Solid
X
X
X
Text
X
X
Shape
X
X
Insert
X
X
Attdef
X
X
Attribute
X
X
Vertex
X
X
Polyline
X
X
X
X
Line3d
X
X
X
X
Face3d
X
X
Entities
X
X
X
Drawing Entities Not Supported
See Table 17-6. Note that the Extrusion, Dimension, and Viewpoint
entities are not supported. Dimensions may be seen on the displayed
DXF file. Some DWG (an AutoCad drawing file) to DXF converters
convert the dimension entities into lines and arcs, which are supported
entities.
17-10
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - DXF Converter Feature
Files Created
The DXF Converter creates the CNC file, .G for G-code and .M for
conversational, or the associated CAM Shape files (.1, .2, etc.) based on
the setting of the Output format parameter.
A file is also created with the extension .fxd. This file saves the status of
parameter settings that were used in Setup.
DXF Example
From the Program listing open the DXF file. Refer to Figure 17-1.
Figure 17-1, Example DXF File
All rights reserved. Subject to change without notice.
17-April-04
17-11
CNC Programming and Operations Manual
P/N 70000487G - DXF Converter Feature
Refer to Figure 17-2. All unneeded layers have been turned off. The
Figure shows the drill locations and the contour selected.
Figure 17-2, Zoomed Part with Unneeded Layers Turned Off
From Figure 17-2, the Output Menu (see Table 17-4, Output Menu
Descriptions) would display as follows:
Table 17-7, Output Menu for Figure 17-2
Output program name . . . .
Shift X. . . . . . . . . . . . . . . . .
Shift Y. . . . . . . . . . . . . . . . .
Output dimensions . . . . . . .
Create Mode. . . . . . . . . . . .
Starting sub number. . . . . .
Output format. . . . . . . . .
Output warnings. . . . . . . . .
Re-calc Intersections. . . . .
Output resolution. . . . . . . .
Create main in new . . . . . .
Convert values. . . . . . . . . .
Convert polyline. . . . . . . . .
17-12
SAMPLE–1
2.41174
6.16598
Absolute
Smart
1
G-Code/ISO
Yes
Yes
5
Yes
None
None
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - DXF Converter Feature
Unedited Conversational Program Listing
The CNC conversational program is created that must be edited to be
usable. An unedited conversational program created from Figure 17-2,
Zoomed Part with Unneeded Layers Turned Off follows. See
Table 17-8.
– or –
An unedited G-code program created from the Figure 17-2 example is
listed in Table 17-9, Unedited G-code Program Listing.
Table 17-8, Unedited Conversational Program Listing
Call 1
Call 2
EndMain
Sub 1
Dim Abs
Rapid
Rapid
Rapid
Rapid
EndSub
X 0.00000 Y 0.00000
X 1.12400 Y 1.37000
X 3.70000 Y 0.00000
X 5.36800 Y 1.37000
Sub 2
Dim Abs
Rapid
X -0.37600 Y -0.25000
Line
X -0.37600 Y 1.62000
Arc Cw X -0.25100 Y 1.74500 Radius 0.12500
Line
X 5.61900 Y 1.74500
Arc Cw X 5.74400 Y 1.62000 Radius 0.12500
Line
X 5.74400 Y 0.37000
Arc Cw X 5.61900 Y 0.24500 Radius 0.12500
Line
X 4.32500 Y 0.24500
Arc Ccw X 4.07500 Y -0.00500 Radius 0.25000
Line
X 4.07500 Y -0.25000
Arc Cw X 3.95000 Y -0.37500 Radius 0.12500
Line
X -0.25100 Y -0.37500
Arc Cw X -0.37600 Y -0.25000 Radius 0.12500
EndSub
The conversational program must be edited to add tool numbers, feed
rates, cutter comp on or off, and so forth. When the edits are complete,
use Draw to check the tool path. See Figure 17-3, Edited G-code Tool
Path.
All rights reserved. Subject to change without notice.
17-April-04
17-13
CNC Programming and Operations Manual
P/N 70000487G - DXF Converter Feature
Unedited G-code Program Listing
The CNC G-code program is created that must be edited to be usable.
An unedited G-code program created from Figure 17-2 Zoomed Part with
Unneeded Layers Turned Off follows. See Table 17-9.
Table 17-9, Unedited G-code Program Listing
M98 P1
M98 P2
M2
O1
G90 G0 X 0.00000 Y 0.00000
G0 X 1.12400 Y 1.37000
G0 X 3.70000 Y 0.00000
G0 X 5.36800 Y 1.37000
M99
O2
G90 G0 X -0.37600 Y -0.25000
G1 X -0.37600 Y 1.62000
G2 X -0.25100 Y 1.74500 R 0.12500
G1 X 5.61900 Y 1.74500
G2 X 5.74400 Y 1.62000 R 0.12500
G1 X 5.74400 Y 0.37000
G2 X 5.61900 Y 0.24500 R 0.12500
G1 X 4.32500 Y 0.24500
G3 X 4.07500 Y -0.00500 R 0.25000
G1 X 4.07500 Y -0.25000
G2 X 3.95000 Y -0.37500 R 0.12500
G1 X -0.25100 Y -0.37500
G2 X -0.37600 Y -0.25000 R 0.12500
M99
The edited program listings are shown in the following Tables:
17-14
q
Table 17-10, Edited Conversational Program Listing
q
Table 17-11, Edited G-code Program Listing
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - DXF Converter Feature
Edited Conversational Program Listing
See Table 17-10.
Table 17-10, Edited Conversational Program Listing
Dim Abs
Unit Inch
Rapid
X -1.0000 Y 0.0000
MCode 5
RPM 2000
Tool# 1
MCode 3
BasicDrill ZDepth -0.6000 StartHgt 0.1000 Feed 20.0
Call 1
DrillOff
Rapid
X -1.0000 Y 0.0000
MCode 5
RPM 1500
Tool# 2
MCode 3
Feed 15.0
Call 2
Rapid
Z 1.0000
MCode 5
EndMain
Sub 1
Dim Abs
Rapid
Rapid
Rapid
Rapid
EndSub
Sub 2
Rapid
X 0.00000 Y 0.00000
X 1.12400 Y 1.37000
X 3.70000 Y 0.00000
X 5.36800 Y 1.37000
Y -0.2500
Z -0.6000
Dim Abs
Rapid
X -0.3760 Y -0.2500 ToolComp Left
Line
X -0.37600 Y 1.62000
Arc Cw X -0.25100 Y 1.74500 Radius 0.12500
Line
X 5.61900 Y 1.74500
Arc Cw X 5.74400 Y 1.62000 Radius 0.12500
Line
X 5.74400 Y 0.37000
Arc Cw X 5.61900 Y 0.24500 Radius 0.12500
Line
X 4.32500 Y 0.24500
Arc Ccw X 4.07500 Y -0.00500 Radius 0.25000
Line
X 4.07500 Y -0.25000
Arc Cw X 3.95000 Y -0.37500 Radius 0.12500
Line
X -0.25100 Y -0.37500
Arc Cw X -0.37600 Y -0.25000 Radius 0.12500
All rights reserved. Subject to change without notice.
17-April-04
17-15
CNC Programming and Operations Manual
P/N 70000487G - DXF Converter Feature
Line
X -1.0000 ToolComp Off
EndSub
Edited G-code Tool Path
The edited G-code tool path is illustrated in Figure 17-3.
Figure 17-3, Edited G-code Tool Path
The edited G-code program used for the Figure 17-3 is listed in
Table 17-11, Edited G-code Program Listing.
17-16
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - DXF Converter Feature
Edited G-code Program Listing
Table 17-11, Edited G-code Program Listing
G90 G70 G0 T0 Z0
* ADD DEFAULTS
X-1 Y0
* MOVE TO START POSITION
M5 S2000
* SPINDLE OFF, SET RPM
T1 M3
* CALL TOOL, START SPINDLE
G81 Z-0.6000 R0.1000 F20.0
* ENABLE DRILL CYCLE
M98 P1
* CALL DRILLING SUB
G80
* DRILLING OFF
G0 X-1 Y0
* RETURN TO START POSITION
M5 S1500
* SPINDLE OFF, SET RPM
T2 M3 F15
* CALL TOOL, START SPINDLE
M98 P2
* CALL COUNTOURING SUB
G0 Z1
* RAPID Z UP
M5
* SPINDLE OFF
M2
* END PROGRAM
O1
G90 G0 X 0.00000 Y 0.00000
G0 X 1.12400 Y 1.37000
G0 X 3.70000 Y 0.00000
G0 X 5.36800 Y 1.37000
M99
* DRILLING SUB
O2
* COUNTOURING SUB
G0 Y-.25
* ADD Y START POSITION
Z-.6
* Z TO CUTTING DEPTH
G41
* COMP TOOL LEFT
G90 G0 X -0.37600 Y -0.25000
G1 X -0.37600 Y 1.62000
G2 X -0.25100 Y 1.74500 R 0.12500
G1 X 5.61900 Y 1.74500
G2 X 5.74400 Y 1.62000 R 0.12500
G1 X 5.74400 Y 0.37000
G2 X 5.61900 Y 0.24500 R 0.12500
G1 X 4.32500 Y 0.24500
G3 X 4.07500 Y -0.00500 R 0.25000
G1 X 4.07500 Y -0.25000
G2 X 3.95000 Y -0.37500 R 0.12500
G1 X -0.25100 Y -0.37500
G2 X -0.37600 Y -0.25000 R 0.12500
G1 G40 X-1
* COMP OFF MOVE
M99
All rights reserved. Subject to change without notice.
17-April-04
17-17
CNC Programming and Operations Manual
P/N 70000487G - DXF Converter Feature
Using DXF for Pockets with Islands (G162)
Refer to “Section 5, Pockets with Islands (G162).” In DXF, make outside
profile shape #1 or lowest number. Then all islands thereafter, the order
is not important. When saving these, use Cam Shape. Refer to
Figure 17-4.
1. Highlight the DXF filename, and press Utility (F9).
2. Highlight DXF Converter, and press ENTER.
3. Press SETUP, select OUTPUT format, press ENTER.
4. Select CAM Shape, and press ENTER. Refer to Figure 17-4.
5. Select to Convert values, and press ENTER.
6. Select Metric, and press ENTER.
7. Press Exit twice.
Figure 17-4, DXF Output format, CAN Shape Pop-up Menu Illustration
Using Figure 17-5, DXF Pockets with Islands Example Workpiece as an
example:
17-18
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - DXF Converter Feature
Figure 17-5, DXF Pockets with Islands Example Workpiece
1. Select a start point on outer profile and make shape #1. A good
point on the workpiece illustrated is just below the radius top left.
2. Select next shape, until all 10 shapes are selected.
3. Press Save (F9), it will save all 10 CAM shapes.
4. Press Exit (F10).
5. Press Yes (F1) to exit.
An AMER3.G program needs to be created. Then the AMER3.G program
is created, a pop-up list of programs is displayed. See Figure 17-6.
Figure 17-6, DXF Program Listing Pop-up Menu Illustration
All rights reserved. Subject to change without notice.
17-April-04
17-19
CNC Programming and Operations Manual
P/N 70000487G - DXF Converter Feature
DXF Program Example
Table 17-12, DXF Pockets with Islands Programming Example
N1
G0 G70 G90
N2
G53 O1
N3
T1
N4
G162 A2 B3 C4 D5 E6
N5
G162 A7 B8 C9 D10
N6
G169
N7
G0 Z2.0
N8
X0.0 Y0.0
N9
M2
The completed DXF Pockets with Islands example is illustrated in
Figure 17-7. The rapid moves are turned off in this illustration.
Figure 17-7, DXF Pockets with Islands Completed Example Workpiece
17-20
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - DXF Converter Feature
Creating CAM Shapes
When “CAM Shape” is selected as the “Output format,” you will need to
know if the input DXF file is formatted in Inch or Metric. (See
Figure 17-4, DXF Output format, CAN Shape Pop-up Menu Illustration.)
If the DXF file is in Metric, you must choose “None” from the “Convert
Values” field. If the DXF file is in Inch format, you must choose “Metric”
from the “Convert Values” field. This is because the CAM is always
expecting Metric input.
Once you have created the shapes in the DXF converter and then saved
them using the F8 (Save) function, you need a “.G” program with the
same name as is listed in the Output menu of the DXF converter. If that
program name does not already exist (See “Section 1, Getting Started”
for program creation from the Program Directory), then go into the CAM
with that “.G” file highlighted. Once in CAM, you press F6 (Misc.) and
select Recover Shapes, then press F5 (Display) and select Fit to view
the CAM shapes.
All rights reserved. Subject to change without notice.
17-April-04
17-21
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Section 18 - CAM Programming
CAM Mode
CAM Mode is very different from the standard G-code method of part
programming. With CAM programming, you create part programs with
the help of icons. These icons prompt you for necessary information.
To use CAM programming, you must know the XYZ (Cartesian)
coordinate system, the polar coordinate system, and machining
sequences. You must make a machining plan, decide which type of tools
to use, and when to use those tools in the program.
You can use CAM programming to generate toolpaths from “shapes.”
These shapes are generated from the icon tools. Icon tools enable the
moves to be put directly into the shapes or create construction geometry.
Construction geometry can then be “chained” to generate moves for the
shapes.
To create the geometric elements required for a part program, such as:
lines, arc, and points, click on the appropriate icon, and press ENTER.
The CNC prompts you to enter a dimension, such as the length of a line
or the radius of an arc. These entries, combined with the Motion (F7)
soft key, enable the system to perform the desired machine sequences.
As you program lines, arcs, and points, they are displayed on the
Graphics screen.
CAM Mode enables you to generate part programs without using Gcodes. Before you use CAM Mode, become familiar with CNC
programming techniques, including G-codes.
Refer to Table 18-1. The CAM Mode screen displays the following
information:
Table 18-1, CAM Mode Screen Displays
XYZ position of the cursor.
Cursor Coordinates
Dimensioning Mode: Absolute or
Abs/Inc Mode Indicator
Incremental.
NOTE: The resulting subprogram will
execute moves using absolute
dimensions.
Inch
or
MM
Mode.
Inch/MM Mode Indicator
Selects specific points for editing.
Cursor
Viewing area.
Display Area
Create and edit shapes.
Drawing Tools
The default soft keys provide tools to
Soft Keys
change the setup, adjust the display, and
manage shapes.
Name of program linked to the shapes.
Program Name
All rights reserved. Subject to change without notice.
17-April-04
18-1
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Pointer Coordinates
Abs/Inc Mode Indicator
Inch/MM Mode Indicator
Pointer
Display Area
Drawing Tools
Soft
Keys
Softkeys
Program Name
Figure 18-1, CAM Mode Screen
CAM Mode Soft Keys
To activate the CAM Mode soft keys:
1. In Manual Mode, press Program (F2) to activate the Program
Directory. Highlight an existing program, then press CAM (F4).
2. The CAM screen activates and the active soft key highlights.
Refer to Table 18-2, CAM Mode Soft Keys.
There are two soft key menus in CAM Mode:
18-2
q
The Main soft key display appears when you enter CAM Mode.
q
The Secondary soft key displays, or Shape (F2) soft keys, are
displayed when you press SHAPE (F2).
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Table 18-2, CAM Mode Soft Keys
Label
Soft Key
SHAPE
S-EDIT
VIEW
F2
F3
F4
DISPLAY
F5
MISC
F6
MOTION
POST
F7
F8
SETUP
F9
Exit
F10
Function
Turns ON Shape soft keys.
Use to create, delete, edit, and import shapes.
Changes the view (XY, XZ, YZ, and ISO). For details
on View, refer to Draw Mode.
Zooms in on an area of a part, scales it to fit the
screen.
Enables you to inspect data relating to shapes and
geometry.
Generates a cutting tool path.
Selects the post-processing function of the CAM
software and creates a G-code program.
Configures the POST processor, turns Shapes, Paths,
and Geometry ON/OFF, sets attributes and switches
between Absolute and Incremental Modes.
Saves all program data and returns to the Program
Directory.
Shape (F2) Soft Keys
From the CAM Mode screen, press Shape (F2). The soft keys
change allowing you to create, delete, edit, and import shapes.
Refer to Table 18-3.
Table 18-3, Shape (F2) Soft Keys
Label
Soft Key
Function
SHAPE
F2
Turns OFF Shape soft keys.
S-EDIT
F3
Use to create, delete, change, and import shapes.
Back
F4
Forw
F5
Prev-S
F6
Moves cursor one step in the opposite direction of the
shape input.
Moves cursor one step forward in the direction of the
shape input.
Moves cursor to the previous shape in the program.
Next-S
F7
Moves cursor to the next shape in the program.
DelMove
F8
Deletes a move from the current shape.
WARNING: If you delete a move other than the
last move of a shape, the previous and next
moves will be connected. To avoid this, move the
cursor to the last move of a shape), then press
DelMove (F8) until the required move is deleted.
DelGeom
F9
Deletes a piece of Construction Geometry from the
current program file.
All rights reserved. Subject to change without notice.
17-April-04
18-3
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Shape Edit Menu
Press S-EDIT (F3) to create a shape, delete a shape, join and project
lines/arcs, merge a shape from another program file (import), and join
elements of a shape. S-EDIT (F3) is displayed in both the main and
secondary, SHAPE (F2) soft key displays to allow you to create a shape
from either display. In S-EDIT, the pop-up displays the following options:
Create, Copy, Move, Delete, Rev Arc, Project, Join, and Import.
IMPORTANT: Before you can program the cursor (described earlier) to
move around a shape using Line, Arc or Chain, you must
first create a shape. To create a shape, program an XY
start position.
Create
Shapes are the basic units of the CAM Mode. They will be used later to
generate the actual tool paths, such as Contour, Pocket. and Drill. When
programming shapes, program the part-edge, or perimeter. The CAM
software will compensate for tool radius when the tool paths are
generated.
To create a shape:
1. Press S-EDIT (F3). Create highlights.
2. Press ENTER. The CNC prompts you to select a point definition tool.
The right-hand column of icons now shows point definitions. Select
one of these to define the XY start position of the shape.
3. After you choose and enter the point definition, the shape cursor is
displayed on the screen at the specified start point. Now you can
program Lines, Arcs, Geometry or Chain moves to make the shape.
In some cases, the part will require you to create more than one shape.
The CNC will automatically number each shape, starting with 1.
For example, you can program the perimeter of a part (Shape 1), to be
contoured later, and then program another shape (Shape 2) to mill a
pocket.
18-4
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Copy
To copy an existing shape:
1. Ensure that the cursor is on the shape.
2. Press S-EDIT (F3). A pop-up activates.
3. Highlight Copy, and press ENTER.
4. The CNC prompts you to Select point definition...
5. Press ENTER. The CNC prompts you to Enter X value: Type the
X-axis start position of the new shape, and press ENTER.
6. The CNC prompts to Enter Y value: Type the Y start position, and
press ENTER.
NOTE: The prompt could be different based on the point definition tool
selected.
7. The new shape displays on the screen. To make changes to the
drawing, press S-EDIT (F3). To deactivate the pop-up, press
DISPLAY (F5). The DISPLAY key is described later in this section.
Move
The Move feature enables you to move a shape to a different location.
To move a shape:
1. Press S-EDIT (F3). A pop-up activates.
2. Highlight Move, and press ENTER.
3. The CNC prompts to Select point definition... Select the first point
definition tool from the right-hand column of the CAM screen.
4. Press ENTER. The CNC prompts to Enter X value: Type the X point
of origin for the new shape, and press ENTER.
NOTE: The prompt could be different based on the point definition tool
selected.
5. The CNC prompts to Enter Y value: Type the Y point of origin for the
new shape, and press ENTER.
6. The new shape displays on the screen. To make changes to the
drawing, press S-EDIT (F3). To deactivate the pop-up, press
DISPLAY (F5). The DISPLAY key is described later in this section.
All rights reserved. Subject to change without notice.
17-April-04
18-5
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Rev Arc
Occasionally, you might program an Arc move in the wrong direction.
Instead of deleting the segment and redrawing it, you can reverse the
Arc’s direction. Arcs at the end of a shape or between any two segments
can be reversed. To reverse an Arc’s direction:
1. Move the cursor to the Arc’s forward node, and press S-Edit (F3).
The S-Edit Pop-Up menu is displayed.
2. Highlight Rev Arc, and press ENTER. The arc will be redrawn in the
reverse direction.
Delete
When necessary, an entire shape can be deleted.
To delete an entire shape:
1. Use Prev-S (F6) and Next-S (F7) to move the cursor to occupy any
node within the shape to be deleted.
2. Press S-EDIT (F3). The S-EDIT Pop-Up Menu displays.
3. Highlight Delete, and press ENTER. The CNC will prompt to confirm
the deletion.
4. Press Yes (F1) or No (F2) as required. Yes causes the shape to be
deleted. No cancels the process.
Sometimes small bits of a shape will remain on the screen after deletion.
Press R, which functions as a hot key, to refresh the screen.
Project
Use the Project feature to remove blend radii and restore the sharp
corners. This operation is called “projecting” because projections are
added to line segments on both sides of a removed radius.
To remove a radius and restore a sharp corner:
1. Move the cursor to the forward node of the radius being removed.
2. Press S-EDIT (F3). The S-EDIT Pop-Up Menu is displayed.
3. Select Project, and press ENTER. The radius will be removed and line
projections forming a sharp angle are added. The editor will prompt
to join the lines.
4. Press Yes (F1) to join the projections. The collinear line segments
are joined into a single straight-line segment.
NOTE: Collinear lines are end-to-end lines that lie in the same direction.
18-6
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Join
Sometimes what appears to be a single line segment is more than one
line segment drawn end-to-end. To detect the presence of the extra
nodes within the segment, move the cursor along the segment.
Collinear segments do not affect the execution of the move. Usually, it is
desirable to join collinear lines to keep the subprogram and future editing
sessions as simple as possible.
Join collinear lines as follows:
1. Position the cursor at the node between the collinear lines.
2. Press S-EDIT (F3). The S-EDIT Pop-Up Menu displays.
3. Highlight Join, and press ENTER. The unnecessary node is removed
from the line.
Import
Sometimes, the same shape is used in more than one program. Instead
of programming the shape more than once, you can import the shape
from its original program.
To import an existing shape from another program:
1. Press S-EDIT (F3). The S-EDIT Pop-Up Menu displays.
2. Highlight Import, and press ENTER. The CNC prompts for the name
of the program containing the shape to be imported.
3. Type the program name, and press ENTER. The CNC displays a list
of the shapes contained in the source program.
4. Highlight the desired shape, and press ENTER. The editor will prompt
to determine if the origin of the shape should be changed.
5. Press Yes (F1) and type a new origin as prompted, or press No (F2)
to import the shape at its original position.
View (F4)
Use the View (F4) function to change the plane view. Options are XY,
XZ, YZ, and Isometric (Iso) views. For details on View, refer to Draw
Mode.
All rights reserved. Subject to change without notice.
17-April-04
18-7
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
MOTION (F7)
Use MOTION to generate tool paths for Contour, Pocket, and Drill
moves. You can use Motion (F7) only after a shape has been input into
the program.
To generate a tool path:
1. From the CAM Mode screen, press MOTION (F7). A pop-up menu
displays. Menu options are: Contour, Pocket, Drill, Edit, and
Delete.
2. Highlight a selection, and press ENTER.
3. Enter cutting parameters so that CAM software can generate a path.
The Calc (calculate) key displays.
4. Press Calc. The CNC calculates the tool path and shows it on the
screen. Choose whether to save the path.
After the toolpath is calculated, press POST (SHIFT+F7) to generate a
CNC program. This program will be a G-code program that the CNC can
use to produce the parts.
Use Edit to change an existing tool path. Use Delete to delete a
toolpath. In all cases, highlighting the field changes parameters, and
pressing ENTER.
Del Move (F8)
DelMove (F8) deletes a move from the current shape. The cursor must
be at the end of the move to be deleted.
WARNING: If you delete a move other than the last move of a
shape, the previous and next moves will be
connected. To avoid this, move the cursor to the last
move of a shape, then press DelMove (F8) until the
required move is deleted.
Contour
Contour highlights when you press MOTION (F7).
Use this feature to cut a profile for:
q
A part perimeter (outline).
q
A perimeter pass to finish a pocket, slot or other type of contour.
The shape does not need to be closed.
Refer to Figure 18-2, Contour Parameters Menu. With Contour
highlighted, press ENTER. Contours Parameters Menu 1 displays.
18-8
All rights reserved. Subject to change without notice.
17-April-04
All rights reserved. Subject to change without notice.
17-April-04
Off
Forw
Rev
None
Off
Forw
Rev
None
Initial move ..........
Coolant at start ....
Coolant at end .....
Feedrate ..............
Z Feedrate ...........
Spindle at start ....
Spindle at end .....
Spindle speed .....
Tool Change .......
2D
None
None
0.0000
0.0000
None
None
0
Machine Setup
No
Off
On
None
Interference check ...........
Tool path color .................
Shape Reversed ..............
Entry Move .......................
Exit Move .........................
Machine setup .................
On
Contour Parameters 2
1
None
0.0000
0.0000
1
0.0000
0.1000
0.0000
0.0000
Toward
Comment .........................
Tool compensation ...........
Tool diameter ...................
XY stepover .....................
Number of XY passes ......
Z step ...............................
Approach height ...............
Top of contour ..................
Bottom of contour ............
Stepover direction ............
More .................................
Contour Parameters 1
Shape number ..................
Off
On
None
2D
3D
Output Tool Change .. No
Tool number .............. 0
Tool Change Configuration
None
Move Type .......
0.0000
Arc Length ........
0.0000
Arc Radius .......
Origin Point .... {0.0000, 0.0000}
Exit Move Setup
None
Linear
Circular
Move Type .......
None
Arc Length ........
0.0000
Arc Radius .......
0.0000
Origin Point .... {0.0000, 0.0000}
Entry Move Setup
Comment ..__
None
Linear
Circular
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Figure 18-2, Contour Parameters Menu
18-9
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Refer to Table 18-4. Contour Parameters 1 Menu lists the following:
Table 18-4, Contour Parameters 1 Menu Options
Parameter
Description and Options
Shape number
Chooses which shape of the program you wish to contour. To enter a
shape, highlight a Shape Number, and press ENTER. Type the number of
the desired shape, and press ENTER.
Tool
Compensation
Chooses the compensation direction. Highlight and press ENTER to
choose CAM left, CAM right, or None. The direction of compensation is
equal to the side of the programmed shape on which the tool is to cut.
View the Left - Right direction in the direction of the first move in the
shape. The end of the first move of each shape has an arrow attached,
which indicates the direction in which the shape was programmed.
Tool diameter
Options:
CAM Left or
CAM Right: The tool path is placed on the appropriate side of the
shape.
None:
No compensation takes place and the tool path equals
the shape.
Enters the tool diameter. Press ENTER to choose Direct or Tool table.
Options:
Direct
Tool table
XY stepover
Enter the tool diameter directly.
The values in the tool table for diameter length only will
be displayed. (Length offsets must be entered at
setup). Highlight a value in the table, and press ENTER
to enter that value into the Tool diameter parameter.
Enters a stepover distance. This parameter applies only if the next
parameter, "Number of XY passes", is programmed to be greater than
one (1). For example: If programmed to 0.0500, and programmed to
three “XY passes” (in next parameter), the tool path is generated with
three complete passes around the profile.
Start point is automatically calculated, based on the start point of the
shape and the compensation value.
This parameter should be 0.0000 if only one pass is required. To set this
parameter, highlight it, press ENTER, and type the tool stepover value.
Number of XY
passes
Makes several passes around a contour. This can be advantageous if a
large amount of stock must be removed, but cannot be taken in a single
pass. If programmed to be greater than one (1), you must also program
XY stepover. To set this parameter, highlight it, type the number of XY
passes, and press ENTER.
(Continued…)
18-10
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Table 18-4, Contour Parameters 1 Menu Options (Continued)
Parameter
Description and Options
Z step
Cuts contour in Z levels. If a contour's depth cannot be machined in one
depth-of-cut, use this to "step" the Z-axis down in levels. It works in
conjunction with the Bottom of contour parameter. For example: if Z
step is set to 0.5000, and the Bottom of contour parameter is set to
-1.0000, the contour will be cut twice (once at Z-0.5000, and once at
Z-1.0000). It is possible to use both XY stepover and Z step for the
same contour path.
Approach
Height
Sets the position to which the Z-axis will rapid before it begins the first
feed move. Generally, if Z0 is set at the top of the workpiece, approach
height is set to 0.1000 inches (0.1 above the part). The default value is
preset to 0.1000. If the top of the workpiece is not Z0, reset this
parameter to ensure a safe, rapid clearance height.
Top of contour
Defines the location of the top of the contour in reference to Z0.
Generally, this is set to 0.0000, but can be set to any value to enable a
contour to be cut at any Z depth.
Bottom of
contour
Sets the final depth of the contour. You must set this parameter to a
value less than the previous parameter (Top of contour) or an Error
message will occur. If the top of the workpiece is Z0, this will be a
negative value.
Stepover
direction
Reverses the XY stepover direction (if programmed) This parameter
refers to the direction in which the stepover will occur. Normally, this will
be toward the shape. Generally, this parameter should be set to
Toward.
Options:
Toward:
Away:
Stepover will occur toward the shape.
The first pass of the sequence will take place next to the
shape, then step away from the shape.
NOTE: This parameter does not apply if only one XY pass is
programmed above.
All rights reserved. Subject to change without notice.
17-April-04
18-11
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Highlight More, and press ENTER to activate the Contour Parameters 2
Menu. Refer to Table 18-5. This menu enables you to set the following
parameters:
Table 18-5, Contour Parameters 2 Menu Options
Parameter
Description and Options
Comment
Enters a comment block into the program. This comment will be output
into the program when you execute the POST function. Refer to POST.
A comment block is not essential, but it can be helpful. If you use a
comment block, * should be the first character, so that CNC will see it as
a comment, not an executable block. Without the * you can enter code
other than a comment.
Interference
check
When ON, forces the CAM software to "look" for tool interference while it
calculates the tool path. Generally, this should be set to the default
setting, ON. Interference could occur if the tool path could not be
calculated with the chosen tool radius.
Options: ON, OFF
Tool path color
Assigns a color to the path that will be generated when you press Calc.
Since more than one path can be generated in a program, it is best to
distinguish one path from another by color. Assign a separate color to
each path to distinguish one from another easily. Press Tool path color
to activate a color bar. To select a tool path color, highlight the color of
choice, and press ENTER.
Options: Choose from color menu.
Shape
Reversed
Sets the path to mill around the shape in the direction opposite to the one
in which the shape was programmed. (For example, CW/CCW).
Each shape has a direction, indicated by an arrow at the end of the first
move of the shape.
NOTE: If set to Tool comp, adjust LEFT or RIGHT accordingly.
Options:
No:
Yes:
The shape is used in the same direction as it was generated.
The shape is used in the opposite direction that it was
generated.
(Continued…)
18-12
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Table 18-5, Contour Parameters 2 Menu Options (Continued)
Parameter
Entry/Exit
Moves
Description and Options
Enters or exits the path with a linear or circular move. If not used, the
tool will plunge in (entry) and Z-out (exit) with the tool directly on the path
of the shape. This is sometimes undesirable, because a tool mark could
be left on the part, especially on the exit move. To eliminate the tool
mark, the entry/exit moves are provided.
Options:
Move Type:
Set whether the move is a line, arc, or if there will be
no entry/exit move (None). Lines require that Entry #4
(origin point) be programmed. Arcs require that
Entries #2 and #3 (arc length, arc radius) are
programmed. None: specifies no entry/exit move.
Arc Length: Determines arc output (90°, 180°, etc.) All arcs are
output tangent to the first/last move of the path. Not
applicable if #1 is set to Linear.
Arc Radius: A radius value for the entry/exit arc. Used only if #1 is
set to Arc. Origin Point: Used only if #1 is set to Linear.
This is the absolute XY dimension to which the "linear"
entry/exit moves go from/to when entering/exiting the
path.
(Continued…)
All rights reserved. Subject to change without notice.
17-April-04
18-13
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Table 18-5, Contour Parameters 2 Menu Options (Continued)
Parameter
Machine setup
Description and Options
Tool change
Enables a tool change and assigns a tool number to the tool that will
machine the contour. This tool number is output to the program with the
POST function. It is not affected by the tool diameter, even if selected
from the Tool Page.
Options:
Initial move:
Output (yes or no) Tool change code will/will not be output to the
program when posted. Set type of tool change (G28
Z, or G0 T0 Z0) in POST settings.
Tool Number: enables a T# to be output to the program when posted.
2D: on the first move of the PATH, the XY axes rapid position first,
then the Z-axis rapid positions to the "Approach height" set
previously. [Default: 2D]
3D: the rapid positioning move will be a 3-axis XYZ move to the start
point.
Coolant at start:
ON
places a coolant ON command in the program before the FIRST
cut in the contour.
Options:
OFF: A coolant OFF command is issued.
NONE: No coolant command will be given. None could be used if
coolant was already issued in a previous contour, or if no coolant
is desired.
Coolant at end:
OFF: Places a Coolant OFF command in the part program after the last
cut in the contour.
ON:
An ON command is issued.
NONE: No coolant command is given.
Feedrate: Enters the cutting feedrate of the contour. Press ENTER to
clear the current value. Type the new value, and press ENTER
to set it.
Z-Feedrate:
Enters the plunge feedrate of the Z-axis. Press ENTER to
clear the current value. Type the new value, and press
ENTER to set it.
(Continued…)
18-14
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Table 18-5, Contour Parameters 2 Menu Options (Continued)
Parameter
Description and Options
Spindle at start:
Spindle at end:
Sets the spindle at the start of the contour. Press
ENTER while the cursor is on the Spindle line to
activate a pop-up that displays options.
Sets the spindle at the end of the contour. Press ENTER
while the cursor is on the Spindle line to activate a
pop-up that displays options.
Options:
OFF, FWD, REV, and NONE. NONE could be used if the spindle was
already turned ON in a previous contour, pocket, or drill menu.
Spindle speed:
Enters direct speed in RPMs into the menu. This is
the speed to which the spindle will be set when you
issue the ON command.
Refer to Table 18-6. Soft Keys in the Contour Menus are as follows:
Table 18-6, Contour Screen Soft Keys
Label
F8
Soft Key
Calc
Function
Calculates and displays tool path. When path is
displayed, the CNC prompts, Save tool path? _.
Yes (F1) saves the path.
No (F2) deletes the path. In either case, all the
parameters of the contour menu(s) will be saved,
until overwritten with new values.
If Yes, the path can still be changed at a later
time/date with the EDIT function of the MOTION
soft key. You can also Delete the path later.
F10
Cont
Backs-up or continues through the windows (until
Calc displays) or to change a previous setting.
NOTE: If your machine tool does not have programmable spindle and
coolant functions, ignore the items that pertain to "Coolant" and
"Spindle."
All rights reserved. Subject to change without notice.
17-April-04
18-15
18-16
0.0000
0.0000
0.0000
0.0000
0.0000
0.0000
0.0000
XY stepover .....................
XY stock ...........................
Z step ...............................
Z stock .............................
Approach height ...............
Top of pocket ..................
Bottom of pocket .. .........
More .................................
Direction of cut .................
Start point ........................
Tool path color .................
Shape Reversed ..............
Entry Move .......................
Exit Move .........................
Machine setup .................
Initial move ..........
Coolant at start ....
Coolant at end .....
Feedrate ..............
Z Feedrate ...........
Spindle at start ....
Spindle at end .....
Spindle speed .....
Tool Change .......
Off
On
None
2D
None
None
0.0000
0.0000
None
None
0
Machine Setup
Forw
Angle of cut ......................
Off
On
None
2D
3D
No
Default
On
Default
Comment .........................
Interference check ...........
Pocket Parameters 2
1
0.0000
Pocket Parameters 1
Shape number ..................
Tool diameter ...................
Off
On
None
None
Move Type .......
0.0000
Arc Length ........
0.0000
Arc Radius .......
Origin Point .... {0.0000, 0.0000}
Output Tool Change .. No
Tool number .............. 0
Exit Move Setup
None
0.0000
Arc Length ........
0.0000
Arc Radius .......
Origin Point .... {0.0000, 0.0000}
Entry Move Setup
Move Type .......
Tool Change Configuration
Default
CAM Point
Default
Angle
Comment ..__
None
Linear
Circular
None
Linear
Circular
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Pocket
Pocket is accessed from the MOTION (F7) Pop-Up. Use it to cut a
pocket of any shape. Pocket shapes must be closed.
Refer to Figure 18-3. In the Motion screen, highlight Pocket, and press
ENTER. The Pocket Parameters Menu is displayed.
Figure 18-3, Pocket Parameter Menus
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Refer to Table 18-7. Pocket Parameters 1 Menu lists the following:
Table 18-7, Pocket Parameters 1 Menu
Parameter
Description and Options
Shape number:
Chooses which shape of the program you wish to contour. To enter a
shape, highlight a Shape Number, and press ENTER. Type the number of
the desired shape, and press ENTER.
Tool diameter:
Enters the tool diameter. Press ENTER to choose Direct or Tool table.
Options:
Direct
Enter the tool diameter directly.
Tool table The values in the tool table for diameter length only will
be displayed. (Length offsets must be entered at setup).
Highlight a value in the table, and press ENTER to enter
that value into the Tool diameter parameter.
XY stepover
Inputs a stepover distance. This parameter is the “width of cut” the tool
will use while it clears the pocket.
XY stock
Leaves extra stock on the perimeter of the pocket, so that a finish pass
can be made using the Contour feature.
NOTE: ANILAM recommends that you leave some amount of XY stock
for a finish pass, then make a contour pass around the
perimeter of the pocket.
To set this parameter, highlight it, press ENTER, type the amount of stock
to be left (per side), and press ENTER.
Z step
Cuts a pocket in Z levels. If a pocket's depth cannot be machined in one
depth-of-cut, use this parameter to "step" the Z-axis down in levels. It
works in conjunction with the Bottom of pocket parameter. For
example: If “Z step” is set to 0.5000, and Bottom of pocket is set to
-1.0000, the pocket will be cut twice (once at Z-0.5000, and once at
Z-1.0000).
Z stock
Leaves extra stock on the bottom of the pocket. If you use this
parameter, you must set up another pocket to reach the final depth.
Approach
height
Sets the position to which the Z-axis will rapid before it begins the first
feed move. Generally, if Z0 is set at the top of the workpiece, approach
height is set to 0.1000 inches (.1 above the part). The default value is
preset to 0.1000. If the top of the workpiece is not Z0, reset this
parameter to ensure a safe, rapid clearance height.
Top of pocket
Defines the location of the top of the pocket in reference to Z0.
Generally, this is set to 0.0000, but can be set to any value to enable a
contour to be cut at any Z depth.
Bottom of
pocket
Sets the final depth of the pocket. You must set this parameter to a
value less than the previous parameter (Top of pocket) or an Error
message will occur. If the top of the workpiece is Z0, this will be a
negative value.
All rights reserved. Subject to change without notice.
17-April-04
18-17
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Table 18-7, Pocket Parameters 1 Menu (Continued)
Parameter
Description and Options
Islands setup
See “Section 5, Pockets with Islands (G162).”
More
Highlight this parameter, and press ENTER to activate Pocket Parameters
2 Menu.
Refer to Table 18-8. This menu enables you to set the following
parameters:
Table 18-8, Pocket Parameters 2 Menu
Parameter
Description and Options
Comment
Enters a comment block into the program. This comment will be output
into the program when you execute the POST function. Refer to POST.
A comment block is not essential, but it can be helpful. If you use a
comment block, * should be the first character, so that CNC will see it as
a comment, not an executable block. Without the * you can enter code
other than a comment.
Interference
Check
When ON, forces the CAM software to "look" for tool interference while it
calculates the tool path. Generally, this should be set to the default
setting, ON. Interference could occur if the tool path could not be
calculated with the chosen tool radius.
Options: ON, OFF
Angle of Cut
Usually set to Default. If so set, the angle of the first cut will be in the
direction of the first element of the shape used for the pocket operation.
The first element of each shape has an arrow at its end that indicates the
direction in which the shape was programmed.
The tool will step over the defined amount (XY stepover), then cut in the
opposite direction, toward the start point. The process will continue until
no further cuts are required.
You can choose to enter the angle of cut, instead of the “Default” option.
To apply a programmed angle, highlight Angle of cut, and press ENTER.
NOTE: Any angle described is in reference to the polar coordinate
system: 0 degrees is the 3-o'clock position (CCW = positive; CW
= negative). In some cases, setting the angle will result in better
pocket clearance, depending on the geometry of the shape used.
Options:
Default:
Angle:
Automatically set the angle of cut.
Enter the angle.
NOTE: If the first element of the shape is an arc, the angle of cut usually
needs to be set.
Some experimentation with the angle may be necessary, to achieve
maximum material removal.
(Continued…)
18-18
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Table 18-8, Pocket Parameters 2 Menu (Continued)
Parameter
Direction of Cut
Description and Options
Describes the direction the tool path will take on its first XY stepover
move after it contacts the programmed Shape.
Options:
Forward:
Reverse:
Start Point
Default:
The first “XY stepover” will be in the direction of the
shape's element the path first contacts.
The tool will move in the opposite direction of the
Shape's element, if possible.
CAM software calculates the start point automatically.
Generally, this point will be at the compensated intersection
of the first and last elements of the shape.
CAM Point
The "points" definition column of icons is displayed. Choose one to define
the CAM Point. The point programmed must lie on or inside the path to
be generated; That is, tool diameter and XY stock (if any) must be taken
into consideration when you program this point.
Use CAM point if you wish to start the machining at a different place
than where the shape was begun.
Other parameters such as Angle of cut and Direction of cut may need
consideration if you select CAM point.
Tool Path Color
Assigns a color to the path that will be generated when you press Calc.
Since more than one path can be generated in a program, it is best to
distinguish one path from another by color. Assign a separate color to
each path to distinguish one from another easily. Press Tool path color
to activate a color bar. To select a tool path color, highlight the color of
choice, and press ENTER.
Options: Choose from color menu.
Shape
Reversed
Sets the path to mill around the shape in the direction opposite to the one
in which the shape was programmed. (For example, CW/CCW).
Each shape has a direction, indicated by an arrow at the end of the first
move of the shape.
NOTE:
Options:
No:
Yes:
If set to Tool comp, adjust LEFT or RIGHT accordingly.
The shape is used in the same direction as it was generated.
The shape is used in the opposite direction that it was
generated.
(Continued…)
All rights reserved. Subject to change without notice.
17-April-04
18-19
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Table 18-8, Pocket Parameters 2 Menu (Continued)
Parameter
Entry / Exit
Moves
Description and Options
Enters or exits the path with a linear or circular move. If not used, the
tool will plunge in (entry) and Z-out (exit) with the tool directly on the path
of the shape. This is sometimes undesirable, because a tool mark could
be left on the part, especially on the exit move. To eliminate the tool
mark, the entry/exit moves are provided.
Options:
Move Type:
Set whether the move is a line, arc, or if there will be
no entry/exit move (None). Lines require that Entry #4
(origin point) be programmed. Arcs require that
Entries #2 & #3 (arc length, arc radius) be
programmed. None: specifies no entry/exit move.
Arc Length: Determines arc output (90°, 180°, etc.) All arcs are
output tangent to the first/last move of the path. Not
applicable if #1 is set to Linear.
Arc Radius: A radius value for the entry/exit arc. Used only if #1 is
set to Arc. Origin Point: Used only if #1 is set to
Linear. This is the absolute XY dimension to which
the "linear" entry/exit moves go from/to when
entering/exiting the path.
Machine Setup
Highlight this parameter, and press ENTER to activate the final Pocket
Parameters Menu. This menu is exactly the same as Contour Menu
Parameters 3.
Pocket Menus Soft Keys
Refer to Table 18-9 for Pocket Menu soft key descriptions.
Table 18-9, Pocket Menus Soft Keys
Label
F8
Soft Key
Calc
Function
Calculates and displays on the screen. After path
is displayed, the CNC prompts: Save tool path? _.
Yes (F1) saves the path.
No (F2) causes the path to be deleted. In either
case, all the parameters of the contour menu(s)
will be saved, until overwritten with new values.
If Yes, the path can still be changed at a later
time/date with the EDIT function of the MOTION
soft key. You can also Delete the path later.
F10
18-20
Cont
Backs-up to previous setting.
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Pockets with Islands (G162)
Refer to “Example #12 Using CAM for Pockets with Islands (G162).”
Drill
Drill highlights when you activate the MOTION (F7) pop-up. Use this
function is to drill holes. A shape must be present in order to use the
Drill function. Holes are be drilled at the end of each separate element
of an open or closed shape.
Many of the parameters in Drill are the same as those in Contour and
Pocket, described previously. Where this is the case, this manual refers
to previous sections.
Refer to Figure 18-4, Drill Parameters Menus. In the MOTION screen,
highlight Drill, and press ENTER. The Drill Parameters Menu 1 displays.
All rights reserved. Subject to change without notice.
17-April-04
18-21
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Drill Parameters 1
Shape number .................
Drill Cycle .........................
Tool diameter ...................
Drill Parameters ...............
Tool path color .................
Machine setup .................
Spot Drilling
Counterboring
Peck Drilling
Tapping
Boring Bi-dir
Boring Uni-dir
Chip Breaker
Flat Bottom
1
0.0000
Spot Drilling Setup
Hole depth......
Start height.....
Return height..
0.0000
0.1000
0.1000
DRILL1
Tool Change Configuration
Machine Setup
Tool Change .......
Initial move ..........
Coolant at start ....
Coolant at end .....
Feedrate ..............
Z Feedrate ...........
Spindle at start ....
Spindle at end .....
Spindle speed .....
2D
None
None
0.0000
0.0000
None
None
0
2D
3D
Output Tool Change .. No
Tool number .............. 0
Off
On
None
Off
On
None
Figure 18-4, Drill Parameters Menus
18-22
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Refer to Table 18-10. This menu enables you to set the following
parameters:
Table 18-10, Drill Parameters 1 Menu
Parameter
Description and Options
Shape number
Chooses which shape of the program you wish to contour. To enter a
shape, highlight a Shape Number, and press ENTER. Type the number of
the desired shape, and press ENTER.
Drill Cycle
Selects a drill-canned cycle to activate in the program. Highlight this
parameter, and press ENTER. A pop-up is displayed that displays all of
the CNC’s canned drilling cycles and a general description of each.
Highlight a drill cycle, and press ENTER. You must set drilling parameters
in the Drill Parameters area of the pop-up.
Options:
Spot Drilling (G81)[Default]
Counterboring (G82)
Peck Drilling (G83)
Tapping (G84)
Boring Bi-dir (G85)
Boring Uni-Dir (G86)
Chip Breaker (G87)
Flat Bottom (G89)
Tool diameter
Enters the tool diameter. Press ENTER to choose Direct or Tool table.
Options:
Direct
Enter the tool diameter directly.
Tool table The values in the tool table for diameter length only will
be displayed. (Length offsets must be entered at setup).
Highlight a value in the table, and press ENTER to enter
that value into the Tool diameter parameter.
NOTE: Drill diameters are generally used only as a reference, as no
diameter compensation is required. ANILAM recommends that
you program a diameter to serve as a reference for every drill.
Drill
Parameters
The Spot Drilling Setup Menu activates. Use this menu to enter all
necessary parameters for the drill cycle selected with the Drill cycle
feature.
Options:
Hole Depth
Start Height
Return Height
Start height and Return height are set to the default value of 0.1000".
(Continued…)
All rights reserved. Subject to change without notice.
17-April-04
18-23
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Table 18-10, Drill Parameters 1 Menu (Continued)
Parameter
Tool path color
Description and Options
Chooses the color that the CNC will use to describe the tool path on the
CRT.
Options:
Choose one of sixteen colors from the pop-up.
Machine setup
Highlight this parameter, and press ENTER to activate the last pop-up
menu in the Drill cycle. All functions in this menu are exactly the same
as those in Contour Parameters Menu 3, with the exception of Feedrate.
The feedrate in Drill Parameters Menu #2 refers to the Z-axis feedrate
output to the drill canned cycle.
Refer to Table 18-9, Pocket Menus Soft Keys. Soft keys and notes on
soft keys in Drill are the same as those in Contour and Pocket.
Edit
Highlight Edit when you press MOTION (F7). Use this function to edit or
change an existing path (Contour, Drill or Pocket operation).
Highlight Edit, and press ENTER. All path numbers for the current
program are shown. They are numbered, beginning with 1, in the order
in which they were programmed, regardless of whether they were
Contour, Drill or Pocket paths. Highlight the desired path number, and
press ENTER.
The parameters for that path will be displayed to enable you to make
changes. After you set the parameter(s), press Calc (F8) to calculate the
new path.
This function enables you to change a toolpath, such as stepover, tool
diameter, spindle speed or path color without having to reprogram all the
parameters.
Delete
Delete is another selection of the MOTION (F7) pop-up. Delete removes
an existing path (Contour, Drill or Pocket) from the program.
Highlight Delete, and press ENTER. All path numbers for the current
program are shown. They are numbered, beginning with 1, in the order in
which they were programmed, regardless of whether they were Contour,
Drill, or Pocket paths. Highlight the desired path number, and press
ENTER. The parameters for that path will be re-displayed to enable you to
make changes. Those paths will be deleted from the program.
18-24
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
POST (F8)
Press POST (F8) in the CAM Mode screen to select the post processing
function of the CAM software. The CNC cannot run a CAM program; it
must create a G-code program from the CAM program. The POST key
will accomplish this task. This is the final step in the CAM programming
process.
Press POST (F8). The CNC automatically creates a G-code file. In most
cases, the program name will already exist (because you created the
program before you entered CAM Mode), and the POST feature will allow
you to overwrite the existing program.
NOTE: Press Setup (F9) to set aspects of the POST processor, such
as Incremental/Absolute output, Inch/MM output, and file
names.
When you have processed the CAM file as a G-code file, press Exit
(F10) to return to the Program Directory. Run the program in Draw
Graphics to test it. Press Select (F6) to load the program. Enter tool
offsets, zero setting, perform dry run(s), and any other machine setup
procedures now, before you run the program to produce parts.
SETUP (F9)
Use SETUP (F9) in the CAM Mode screen to configure the POST
processor; turn SHAPES, PATHS, and GEOMETRY ON/OFF; set
attributes such as arrows ON/OFF, labels, axes lines, and axes grid
ON/OFF. SETUP also allows you to switch between Absolute and
Incremental programming. You can set the screen to show only the
Paths, Shapes, and Geometry desired. This minimizes screen clutter.
Refer to Table 18-11. In the SETUP (F9) menu, highlight Settings to
determine how the image on the screen will appear.
Table 18-11, Setup Options Settings
Parameter
Dimensions
Description and Options
Dimensions are in reference to Absolute zero, or where the XY axes
intersect. For angles, 0 degrees is the 3 o'clock position. Positive
degrees is CCW.
Incremental dimensions are dimensions in reference to the current shape
cursor position. Each position can be considered a new "zero point"
when programming in Incremental. For angles, 0 degrees is the point
reference.
Options:
Absolute
Incremental
(Continued…)
All rights reserved. Subject to change without notice.
17-April-04
18-25
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Table 18-11, Setup Options Settings (Continued)
Parameter
Input Units
Arrows
Labels
Axes
Grid
Grid Size
Description and Options
Switches modes while programming. The G-code output by the POST is
not affected by this setting.
Options:
Inch
Millimeter
Turns ON/OFF the arrows that display on the first move of any shape.
Arrows indicate the direction of the shape.
Options:
ON [Default]
OFF
Turns ON/OFF the labels that appear with each shape, path, and
geometry element. The labels refer to the numbers of each shape, path,
or geometry element (1, 2, 3, etc.).
Options:
ON [Default]
OFF
Turns ON/OFF the axes lines (X,Y,Z).
Options:
ON [Default]
OFF
Sets the Grid ON/OFF. When ON, the grid displays at the spacing
defined in the next parameter (Length). The grid displays as either dots
or solid lines, depending on the parameter in the CNC Setup Utility. Grid
does not appear in Iso view.
Sets grid spacing.
Shapes
Shapes, an option in the SETUP (F9) pop-up, turns off programmed
shapes. Highlight Shapes, and press ENTER. A pop-up displays the
shape numbers. Highlight the desired shape number, and press ENTER.
The shape will be removed from the display. It is not deleted, only
removed from view. To restore a shape to the screen, turn it ON.
18-26
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Paths
Paths, an option in the SETUP (F9) pop-up, turns off programmed paths.
Highlight Paths, and press ENTER. A pop-up displays the path numbers.
Highlight the desired path number, and press ENTER.
The path will not be deleted, only hidden. To restore a path to the
screen, turn it ON.
IMPORTANT:
If a Path is turned OFF when the POST function is
executed, that path will not appear in the G-code
program. Therefore, you can eliminate a path from the
program without deleting.
Geometry
The Geometry setting in the SETUP (F9) pop-up enables you to turn
OFF construction geometry by groups. Highlight Geometry, and press
ENTER. Refer to Table 18-12. If construction geometry exists, a pop-up
displays the following options:
Table 18-12, Geometry Options
All
Lines
Circles
Points
Construction geometry turns ON/OFF (points. lines. and
circles).
Only construction geometry lines turn ON/OFF.
Only construction geometry circles turn ON/OFF.
Only construction geometry points turn ON/OFF.
After you have used the Chain function on the existing construction
geometry, you may delete all or some elements. This allows a clearer
view for path programming (Contours, Pockets, Drills). When turned
OFF the construction geometry is not deleted, only removed from the
screen. To restore construction geometry, turn ON the above elements.
Post (F8)
Refer to Figure 18-5, POST Menu Options and Table 18-13, POST Menu
Options. Press POST (F8) to configure the POST processor with the
following settings:
All rights reserved. Subject to change without notice.
17-April-04
18-27
18-28
Yes
Abs
Inch
Suppress
On
1
Minimum.................................
Maximum................................
Zero Fill..................................
Yes
No
Repeat
Suppress
8
8
No
Decimal Format Configuration
Overwrite File ...........
Dimensions ..............
Output Units .............
Axes .........................
Text ..........................
Program Number .....
Block Numbers ........
Tool Change ............
Format .....................
G-Code Configuration
G-Code File Name ...
4AX-DRL.G
Block Numbers
MM
Inch
{0.0000, 0.0000}
0.0000
T%02d
0.0000
Yes
Z Position .....
Home Z .....
Tool Change Z Location
Output Z Location .....
Z Location ..................
Tool Change Z Location Setup
XY Location ..............
Z Location ..................
Tool change format ....
Tool Change Configuration
Output Block Numbers .. Yes
Starting ..........................
10
Increment ....................... 10
Off
On
Abs
Inccr
POST1
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Figure 18-5, POST Menu Options
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Table 18-13, POST Menu Options
Parameter
G-code
filename
Overwrite file
Dimensions
Output units
Description and Options
Enters a new file name to which you can output G-code.
The default name is the one highlighted when you entered CAM Mode.
Refer to Contour.
Options:
No: Enables the CNC to prompt for overwriting when you press
POST (F8).
Yes: The existing .G file will be automatically overwritten.
[Default: Yes].
Sets G-code output.
Options:
Absolute or Incremental dimensions. [Default: Absolute]
Sets G-code output.
Options:
Inch or Millimeter. [Default: MM]
Modal
The CNC can Suppress or Repeat G-code output data (axes positions
only)
Options:
Set to Repeat, if two sequential points have the same X or Y dimension.
Both dimensions will always be output. [Default: Suppress]
Text
The CNC can prevent the G-code text from showing on the screen when
you initiate POST.
Options:
On, Off [Default: On]
Selects a program number. This is the "0" that displays when you initiate
POST. This feature is not a requirement.
Program
number
Block
numbers
The CNC can output block (N) numbers to the G-code file, and set their
increments. Highlight Block numbers, and press ENTER. A pop-up displays
with the parameters Output Block Numbers, Starting and Increment.
Options:
[Default Settings: Yes, 10,10]
Tool change
Selects the type and location of the tool change. (Set Yes or No for tool
change in the "Machine Setup Menus of Contour, Pocket, and Drill.”)
Highlight Tool change, and press ENTER. A pop-up displays: XY location
is the location of the tool change. This value displays before each tool
change.
Options:
[Default Setting: X0 Y0] Z Location specifies where/how Z-AXIS will be
handled during tool change. If set to HOME Z, the CNC will output a G28 Z
to the G-code file. If set to Z Location, a T0 and the location given, (usually
0) will be output to the G-code file.
(Continued…)
All rights reserved. Subject to change without notice.
17-April-04
18-29
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Table 18-13, POST Menu Options (Continued)
Parameter
Format
Description and Options
Selects the minimum and maximum number of decimal places, and to
specify if Zero-fill is ON or OFF.
NOTE: ANILAM recommends that you set the maximum number of
decimal places to at least eight places. Zero fill specifies whether
or not leading/trailing zeros will occur.
[Default Settings: 8, 8, No]
If a path is OFF during the POST function, the CNC will not output that
path to the G-code file. In this way, a path can be eliminated from the
output file without actually deleting it from the CAM program.
NOTE: Ensure that all paths you need for the G-code program turn ON.
NOTE: These parameters can be set as a default by copying the “.cam”
file in the c:\user\ directory to the c:\p6m\ directory renaming the
file to defaults.cam.
Posting Output Automatic Tool Changes
The following instructions modify the CAM post processor to output the
automatic tool changes.
1. Enter CAM mode.
2. Select F9 Set Up.
3. Select Post.
4. If M06 is required for a tool change, cursor down to Tool. It will
read T%02d as a default. Change this to read T%02dM06.
5. If there are any other changes the user would like to make to the
post processor, such as number of decimal places output, these
can also be changed at this time.
6. Exit the post processor settings by pressing F10 twice, and then
F9.
7. With the cursor, highlight the .Cam file that has just been
generated.
8. Select F9 Utilities, then Copy
9. Go to Other, type C:\P6M\DEFAULTS.CAM then press ENTER.
10. CAM mode should now use the new defaults when post
processing.
Manual machines use only "T1" or "T5" to call for a tool change. This
stops the machine on this tool number so that the operator can insert a
new tool into the spindle.
18-30
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Automatic tool changing machines typically require that "M6" be added to
the tool line. For example: "T1 M6" or "T5 M6"
This "T1" tells the machine that a new tool is going to be used, and the
"M6" tells it to run the macro and get the tool automatically.
Exit (F10)
After you finish the CAM program and have used the POST function
described above to create a G-code program, press Exit (F10) to save all
program data. The CNC returns to the Program Directory. Press Exit to
leave CAM Mode. If you select CAM again, with the same program
highlighted, all data is restored.
NOTE: Press Quit (SHIFT + F10) to exit without saving changes.
If all aspects of a program are to be deleted, press SHIFT+F3 in the
Program screen, then type Program.*. The CNC prompts for file
deletion. This feature enables certain files to be saved, if desired.
Hot Keys
Hot Keys are available in CAM Mode, if you are using a PC keyboard on
the CNC or the off-line software. Refer to Table 18-14.
Table 18-14, Hot Keys in CAM Mode
Hot Key
A
D
H
W
M
R
ALT + X
ALT + Y
ALT + Z
U
ALT + O
Function
Auto Fit (zoom)
Double size
Half size
Window
Absolute/Incremental switch
Redraw
XY view
YZ view
ZX view
Unit switch
Iso view
All rights reserved. Subject to change without notice.
17-April-04
18-31
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Using the Shape Cursor
You can position the shape cursor only on nodes or endpoints. Use the
cursor to select items.
The forward end of a shape is the end away from the origin (starting
point). The origin is always the back endpoint of the shape. Use Back
(F4) and Forw (F5) SHAPE (- and + keys respectively on off-line
keyboards) to move the cursor from node to node along a shape.
The shape cursor must be positioned at the forward end of a shape to
add a segment. Shape segments cannot be added to the back end of a
shape. Use the cursor to select nodes for chamfering, rounding or
deleting.
Selecting Editing Tools
Use editing tools to create or edit shapes. Select an editing tool from the
two columns of templates. Templates in the left column determine a new
segment’s shape. Templates in the right column determine how the new
segment will be created.
Templates use a standard convention to describe moves. Each template
depicts a segment with a hollow circle at one end and a solid circle at the
other. The solid circle represents the cursor. The hollow circle is the
endpoint of the segment being added. CAM Mode prompts for the letter
values shown in Table 18-15.
Table 18-15, Template Lettering Conventions
Letter
Definition
X
X-axis endpoint (usually a diameter).
Y
X-axis endpoint (usually a diameter).
I
X-axis coordinate of a circle or radius center.
J
Y-axis coordinate of a circle or radius center.
R
Radius value
A
An included or absolute angle.
C
Circle
D
Distance
Refer to Figure 18-6, Shape Editing Tools. To select the shape of a new
segment, use ARROWS to move up and down the left column of
templates. After you highlight the desired shape, use the right arrow to
select the method by which to define the new segment. Only the line and
the arc have more than one description method. (The Geometry tool is
described later.)
18-32
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Figure 18-6, Shape Editing Tools
The Line tool and the Arc tool are used to rough out the main features of
the shape. After you have drawn the major features, go over the shape
and add chamfers and corner rounding, as needed.
Line Tools
In addition to the six templates in the right column, the endpoint of a line
can be described with endpoint definition tools. To select this option,
highlight the Line template, and press ENTER. This activates the point
definition templates, displayed in the right template column. Refer to
Table 18-16, Line Segment Tools and Table 18-18, Line Segment
Endpoint Definition Tools.
All rights reserved. Subject to change without notice.
17-April-04
18-33
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Table 18-16, Line Segment Tools
Line Segment
Template
Line Definition Templates
Use absolute or
incremental X-axis
endpoint.
L
RIGHT ARROW
enables use of
these line definition
templates.
Values Required
LINE from cursor to endpoint parallel to X-axis.
Defined by X POSITION.
Use absolute or
incremental Y-axis
endpoint.
Line from cursor to endpoint PARALLEL to Y-axis.
Defined by Y position.
LINE from cursor to endpoint in any direction.
Defined BY X Y endpoint.
Use absolute or
incremental X and
Y-axis coordinates
to define endpoint.
Use radius and
absolute angle.
Line from cursor to endpoint in any direction.
Defined by radius and angle (polar coordinates).
Use absolute X
position and angle.
Line FROM cursor to endpoint in ANY direction.
Defined by X endpoint coordinate and absolute
angle.
Use absolute Y
position and angle.
LINE from cursor to endpoint in any direction.
Defined by Y endpoint COORDINATE and absolute
angle.
18-34
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Table 18-17, Line Segment Endpoint Definition Tools
Template
Purpose
X, Y
Press ENTER to
activate these
point definition
templates.
Geometry
elements can be
used as a
reference.
Requirements
Use absolute X and Y
position of the point.
Defines a point in an X and Y coordinate
system.
Use incremental X and
Y distance from existing
point.
Defines a point at X and Y increment from
existing point.
Defines a point at radius and angle from
existing point.
Use distance from
existing point and
number of degrees from
3 o’clock position.
Use center of existing
circle.
Identifies the center point of an existing circle.
Use one intersection
point between two
elements.
Identifies the intersection points of any two
elements in the geometry. Prompts to select
a point when more than one intersecting point
exists.
Use existing point.
Identifies existing points. Usually used when
construction of other element requires a
reference point.
All rights reserved. Subject to change without notice.
17-April-04
18-35
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Arc Tools
Refer to Table 18-18. There are two types of Arcs: clockwise (Cw) and
counterclockwise (Ccw). Press ENTER while the icon is highlighted to
switch arc segment direction. Use RIGHT ARROW to access the definition
templates. Use UP/DOWN ARROW to select.
Table 18-18, Arc Segment Tools
Arc Template
Arc Definition Template
Arc from cursor to endpoint. Endpoint and
center keyed in by operator.
Press ENTER to
switch BETWEEN
clockwise (Cw) and
COUNTERCLOCKWISE
(Ccw).
Arc from cursor to endpoint. Endpoint and radius
keyed in by operator. Center calculated by CNC.
Arc from cursor to endpoint. Center and
included angle keyed in by operator. Endpoint
calculated by CNC.
Tangent arc from cursor to endpoint. Endpoint
and radius keyed in by operator. Center is
calculated by CNC. Center and radius values
must be correct for tangent arc.
Line from cursor followed by tangent arc. Line
direction defined by the angle. Arc defined by X,
Y endpoint and radius. Arc starts where tangent
to line from cursor.
Arc followed by tangent line from cursor to
endpoint. Line is defined from cursor to X, Y
endpoint. Arc from cursor to tangent intersection
with line is defined by radius.
18-36
Values Required
Use absolute or
incremental X, Y to
define endpoint.
Use absolute or
incremental I, J to
define center.
Use radius and
absolute or
incremental X, Y
endpoint.
Use absolute or
incremental I, J
centerpoint. Use
incremental angle.
Use incremental
radius and
absolute or
incremental X, Y
endpoint.
Use radius and
absolute or
incremental X, Y
endpoint.
Use absolute
angle.
Use radius and
absolute or
incremental X, Y
endpoint.
Use absolute
angle.
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Corner Radius
The corner radius tool enables you to insert a corner radius segment in
place of the sharp corner at the node between two segments.
To round a corner:
1. Move the cursor to the corner being rounded.
2. Highlight the Rounding
prompt for the blend radius.
icon, and press ENTER. The CNC will
3. Type the blend radius, and press ENTER. A new radius segment will
be inserted in place of the original corner.
NOTE: Rounding can be performed only on a node located between
two shape segments. The forward end or back end of a shape
cannot be rounded.
Chamfering Corners
The Chamfering tool enables you to chamfer selected corners on the
shape.
To chamfer a corner:
1. Move the cursor to the node to be chamfered.
icon, and press ENTER. The CNC
2. Highlight the Chamfering
will prompt for the chamfer distance.
3. Type the desired chamfer distance, and press ENTER. A new line
segment chamfering the corner will be added to the shape in place of
the original corner.
NOTE: Chamfering can be performed only on a node located between
two shape segments. The start or end of a shape cannot be
chamfered.
Shape Edit Soft Keys
The following tasks are described in this topic:
q
q
q
q
q
q
q
q
Reversing an Arc’s Direction
Deleting a Shape
Projecting Line Segments (Restoring Sharp Corners)
Joining Line Segments
Importing Shapes from Other Programs
Deleting a Segment
Changing the CAM Mode View
Viewing a Listing of Shape Segment Details
All rights reserved. Subject to change without notice.
17-April-04
18-37
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Reversing an Arc’s Direction
Occasionally, you might program an arc move in the wrong direction.
Instead of deleting the segment and redrawing it, you can reverse the
arc’s direction. Arcs at the end of a shape or between any two segments
can be reversed. To reverse an arc’s direction:
1. Move the cursor to the arc’s forward node and press S-Edit (F3).
The S-Edit Pop-Up menu is displayed.
2. Highlight Rev Arc, and press ENTER. The arc will be redrawn in the
reverse direction.
Deleting a Shape
When necessary, you can delete an entire shape. To delete an entire
shape:
1. Use Prev-S (F6) and Next-S (F7) to move the cursor to occupy any
node within the shape to be deleted.
2. Press S-Edit (F3). The S-Edit Pop-Up menu displays.
3. Highlight Delete, and press ENTER. The CNC prompts to confirm the
deletion.
4. Press Yes (F1) or No (F2) as required. Yes causes the shape to be
deleted. No cancels the process.
Projecting Line Segments (Restoring Sharp Corners)
Use the Project feature to remove blend radii and restore the sharp
corners. This operation is called “projecting” because projections are
added to line segments on both sides of a removed radius.
To remove a radius and restore a sharp corner:
1. Move the cursor to the forward node of the radius being removed.
2. Press S-Edit (F3). The S-Edit Pop-Up menu displays.
3. Select Project, and press ENTER. The radius will be removed and line
projections forming a right angle are added. The editor prompts you
to join the lines.
4. Press Yes (F1) to join the projections. The collinear line segments
are joined into a single straight-line segment.
NOTE: Collinear lines are end-to-end lines that lie in the same direction.
18-38
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Joining Line Segments
Sometimes, what appears to be a single line segment is more than one
line segment drawn end-to-end. To detect the presence of the extra
nodes within the segment, move the cursor along the segment.
Collinear segments do not affect the execution of the move. Usually, it is
desirable to join collinear lines in order to keep the program and future
editing session as simple as possible.
Join collinear lines as follows:
1. Position the cursor at the node between the collinear lines.
2. Press S-Edit (F3). The S-Edit Pop-Up menu displays.
3. Highlight Join, and press ENTER. The unnecessary node is removed
from the line.
Importing Shapes from Other Programs
Sometimes, the same shape is used in more than one program. Instead
of programming the shape more than once, you can import the shape
from its original program.
To import an existing shape from another program:
1. Press S-Edit (F3). The S-Edit Pop-Up menu displays.
2. Highlight Import, and press ENTER. The CNC prompts for the name
of the program containing the shape to be imported.
3. Type the program name, and press ENTER. The CNC displays a list
of the shapes contained in the source program.
4. Highlight the desired shape, and press ENTER. The editor prompts
you to determine if the origin of the shape should be changed.
5. Press Yes (F1) and type a new origin as prompted or press No (F2)
to import the shape at its original position.
Deleting a Segment
You can delete segments from an end or the middle of a shape. When a
segment is deleted, the node marked by the cursor and the preceding
segment is removed. When a segment is deleted from the middle of the
shape, the segment in front of the cursor is reconnected to the preceding
node.
To delete the segment at the forward end of the shape:
1. Move the cursor to the forward end of the shape.
2. Press DelMove (F8), and press ENTER. The last shape on the
segment is removed.
NOTE: Sometimes, small bits of a deleted shape remain on the screen.
Press R, which functions as a hot key, to refresh the screen.
All rights reserved. Subject to change without notice.
17-April-04
18-39
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Changing the CAM Mode View
Press DISPLAY (F5) to access the following display functions.
q
q
q
q
q
q
q
Fit
Window
Half
Double
Scale
Pan
Erase
These functions perform the same operations described in the Draw
Mode. Refer to “Section 8 - Viewing Programs with Draw.”
Viewing a Listing of Shape Segment Details
To view the details of the moves in any shape:
1. Refer to Table 18-19.
2. Press MISC (F6). The MISC Pop-Up Menu is displayed with the
following options:
Table 18-19, Miscellaneous (F6) Soft Keys
Soft Key
Shapes
List
Description
Shows selected shape’s data. If more than one shape
exists, select the desired shape number. The data
displayed is for the lines and arcs that comprise the shape.
The following data is displayed:
q
Shape starting point.
q
Lines: the X, Y endpoint and length for each line,
respectively.
q
Arcs: the direction (CW or CCW), endpoint, center
point, and radius for each arc.
Press Cancel (F9) or ENTER to return to the main CAM soft
keys.
Geometry Shows Construction Geometry data for construction points,
lines and circles that have been programmed, including:
List
q Points: X and Y positions, respectively.
q Lines: the X intersection (Xin), Y intersection (Yin) and
angle for each line. The line is unbounded geometry
(infinitely long). Therefore, the point at which it
intersects each axis is given (Xin, Yin). If the line is
parallel to an axis, it is called Vertical or Horizontal, and
the X dimension or Y dimension is displayed.
(Continued…)
18-40
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Soft Key
Calc
Distance
Recover
Shapes
Description
q Circles: the center point and radius for each circle.
Press Cancel (F9) or ENTER to return to the main CAM soft
key display.
NOTE: The number of each geometric element is
displayed in the Display Area in the order in which
they were programmed.
Calculates and displays the shortest distance between any
two elements on the tool path. Enter the first and second
elements at the prompt.
Enables shapes to be recovered if the .CAM file has been
deleted. In CAM Mode, while the cursor is on the (.G)
filename in the directory, the CNC automatically creates
special files. The .CAM extension (and file of same NAME)
file holds data related to shapes, but not the shapes
themselves. If the .CAM file was deleted, recovery of the
actual paths is possible only via this function. Use only if
the .CAM file has been deleted and you wish to recover the
shapes. If no recovery is possible, a message is displayed.
Additionally, this feature can be used to import a series of
DXF shapes that were saved as CAM Shapes. Refer to
“Section 17 - DXF Converter Feature” for more details.
Recover
Paths
Enables paths to be recovered if the .CAM file has been
deleted. In CAM Mode, while the cursor is on the (.G)
filename in the directory, the CNC automatically creates
special files. The .CAM extension (and file of same NAME)
file holds data related to paths, but not the paths
themselves. If the .CAM file was deleted, recovery of the
actual paths is possible only via this function.
Use only if the .CAM file has been deleted and you wish to
recover the paths. If no recovery is possible, a message is
displayed.
Press Misc (F6). The Misc Pop-Up menu displays.
1. Shapes List is highlighted by default. Press ENTER. The list of the
shapes available in the file displays.
2. Highlight the shape to be viewed, and press ENTER. The details of the
moves in the shape appear in a box on the screen.
The following details are presented:
q
q
q
Starting point (origin)
Line endpoint and lengths
Arc directions, centers, and radius
All rights reserved. Subject to change without notice.
17-April-04
18-41
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Using Construction Geometry
Points, lines, and circles are the basic elements of all construction
geometry. Use construction geometry to find path intersections not given
on the blueprint. construction geometry can also eliminate the need for
many trigonometric functions.
The geometry of a shape can be constructed on the screen with
geometry tools. After the tool path is solved, the intersecting segments of
the geometry are chained together to form a shape.
Construction geometry is useful when you work with blueprints that
contain limited information. Many combinations of geometry can be
entered to help you find intersections.
Accessing Geometry Tools
To access the Geometry tools:
1. Move the left column highlight to select the GEOMETRY
icon.
2. Press ENTER to cycle through the right column’s three sets of
geometry icons. When the desired icons are displayed, use RIGHT
ARROW to highlight an icon in the right column.
3. Highlight the desired tool, and press ENTER.
Points, lines, and circles can be defined in several ways. Each geometry
tool defines a geometry element differently. A tool that requires a point
position to start will prompt to select and activate an additional point
definition tool.
Lines and circles are drawn on the screen with dotted lines. Points are
marked by Xs. All geometry elements are numbered.
Geometry tools generally produce one of the three different elements.
Review the table listings to understand Geometry tools. Some tools
require that certain elements be part of the geometry. ANILAM
recommends that first-time operators experiment with all of the drawing
tools. The following tables are provided as a reference to the features of
each tool. Look over each of the tables before you attempt the
examples.
18-42
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Point Tools
Some point tools define the position of a point in the coordinate system,
others allow you to select an existing point in the geometry. Refer to
Table 18-20.
When you use tools that require a starting point, a through point, or a
from/to point, the Shape Editor displays the “Select point definition . . .,”
message. You must then activate an additional point tool and define the
required point.
Tools that identify centerpoints or element intersections will prompt for
necessary element numbers, highlight all possible points, and prompt you
to select one.
Table 18-20, Geometry Point Tools
Template
Purpose
Requirements
Defines a point in a geometry.
q
Must know absolute X and Y
position of the point.
Defines a point at X & Y
increment from existing point.
q
One endpoint must already be
an element of the geometry.
q
Must know incremental X and Y
distance from existing point.
q
One endpoint must already be
an element of the geometry.
q
Must know distance from
existing point.
q
Must know number of degrees
from 3 o’clock position.
Identifies the centerpoint of an
existing circle.
q
The circle must already be an
element of the geometry.
Identifies the intersection points of
any two elements in the
geometry. Prompts you to select
a point when more than one
intersecting point exists.
q
Geometry must already contain
an intersection of two elements.
Identifies existing points, usually
used when construction of other
element requires a reference
point.
q
Desired point must already be
an element of the geometry.
Defines a point at radius and
angle from existing point.
All rights reserved. Subject to change without notice.
17-April-04
18-43
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Line Tools
Some Line tools require point definition or identification to start. Refer to
Table 18-21. The CAM Mode displays a message when this is
necessary. Line tools that draw tangents to circles display all possible
lines and prompt to select one.
Table 18-21, Geometry Line Tools
Template
18-44
Purpose
Requirements
Constructs a line parallel to
Y-axis, at given X position.
Prompts for X value.
q
Must know absolute position the
line crosses the X-axis.
Constructs a line parallel to
X-axis, at given Y position.
Prompts for Y value.
q
Must know absolute position the
line crosses the Y-axis.
Constructs a line between any
two points. Prompts to select
any convenient point tool when
activated.
q
Use any method to locate the two
endpoints.
Constructs a line through a point,
rotated specified number of
degrees from 3 o’clock position.
Prompts to select any point tool
to define point.
q
Must know angle.
q
Use any method to locate point of
rotation.
Constructs line parallel to
existing line at specified (positive
or negative) distance.
q
Line must already be an element
of the geometry.
Constructs line tangent to circle
that passes through selected
point. Prompts to select any
point tool. Always draws tangent
lines to both sides of circle, you
must select one.
q
Circle must already be an element
of the geometry.
q
Use any method to locate the
point.
Constructs line tangent to any
two circles. Always draws the
four possible lines, you must
select one.
q
Two circles must already be
elements of the geometry.
Constructs line rotated specified
number of degrees from 3
o’clock position and tangent to
existing circle.
q
Circle must already be an element
of the geometry.
q
Must know number of degrees of
rotation from 3 o’clock position.
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Circle Tools
Some circle tools require point definition or identification when used.
Refer to Table 18-22. The CAM Mode displays a message when this is
necessary. Circle tools that draw circles tangent to other circles, lines, or
points construct all possible circles and then prompt you to select one.
Table 18-22, Geometry Circle Tools
Template
Purpose
Requirements
Constructs circle of specified
radius tangent to any two points,
lines or circles. Draws all
possible solutions; you must
select one.
q
Geometry must contain at least
two elements.
Constructs circle of specified
radius centered at any position.
Prompts to select any point tool
to define circle center point.
q
Use any method to locate center
point.
q
Must know radius.
Constructs circle of specified
radius tangent to line and point.
Prompts to select any point tool
to define point.
q
Line must already be an element
of the geometry.
Constructs circle tangent to line
with center at defined point.
Prompts to select any point tool
to define centerpoint.
q
Line must already be an element
of the geometry.
q
Use any method to locate center
point.
Notes on Geometry
Access all geometry tools with the left column geometry icon
highlighted. When the template is highlighted, press ENTER to cycle the
right column through three sets of the Geometry Tool templates.
Construct geometry so that each node of the required shape is an
intersection of two geometry elements.
All rights reserved. Subject to change without notice.
17-April-04
18-45
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Chaining Geometry Elements to Create a Shape
You must create a shape before chaining can occur. The shape starting
point (origin) should be a point on an element of the construction
geometry. The new shape will be chained, from the starting point, around
various geometry elements.
icon, and press ENTER. The CNC prompts to
Highlight the CHAIN
“Select element:”. Type a sequence of intersecting geometry elements
by number, each separated by a space. Press ENTER. The CNC traces
the new shape from intersection to intersection. Each intersection will
become a node in the shape.
The path around a circular Geometry element can be either in a
clockwise or counter clockwise direction.
If the intersecting Geometry element is a circle, a positive element
number creates a counterclockwise path, a negative element number
creates a clockwise path.
If the direction of the path around any element is incorrectly chained, the
direction can always be reversed with the shape editing tools. Elements
can be chained one at a time or all at once.
Viewing a Listing of Geometry Elements
A complete listing of all the Geometry elements and relevant position
information is available.
To view the Geometry list:
1. From the default soft key line press MISC (F6). A pop-up menu
displays.
2. Highlight Geometry List, and press ENTER. A listing of geometry
elements and position data displays.
The following information is displayed:
18-46
q
Element number
q
Points - X and Y positions
q
Lines parallel to X-axis – Y-axis position
q
Lines parallel to Y-axis – X-axis position
q
Lines through a point - point position and angle
q
Circles - The center point and radius
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Deleting Geometry Elements
After a shape has been chained together from Construction Geometry,
the geometry can be deleted, if desired. Elements can be left in the
program along with the shape.
To delete geometry elements:
1. Press DelGeom (F9). The CNC prompts for the number of the
geometry element to be deleted.
2. Type the element number, and press ENTER. The element is removed
from the display.
Sometimes, small bits of an element will remain on the screen after
deletion. Press R, which functions as a hot key, to refresh the screen.
NOTE: Deleted geometry cannot be restored.
Deleting All Geometry Elements
To delete all geometry elements:
1. With the SHAPE soft keys active, press SHIFT and DelAll (F9). The
CNC prompts to confirm deletion.
2. Press Yes (F1) to delete or No (F2) to cancel.
Sometimes, small bits of a deleted element remain on the screen after
deletion. Press R, which functions as a hot key, to refresh the screen.
NOTE: Deleted geometry cannot be undeleted.
Managing Shape Files
The CNC automatically name files created in CAM Mode. Files contain
the same primary name as the G-code file with which they are
associated. The CNC generates several files with the G-code file but
different extensions. These file extensions are:
q
FILENAME.CAM - CAM mode settings
q
FILENAME.GEO - Construction Geometry
q
FILENAME.1 - (or .2, .3) are Shapes
q
FILENAME.$* - Temporary files
q
FILENAME.T (number) are toolpaths backup files
All rights reserved. Subject to change without notice.
17-April-04
18-47
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Using Shapes In G-code Programs
You can use any shapes that you create in CAM in G-code programs.
Anywhere you can use a subprogram in a G-code program, you can also
use a shape. For example, the W address in G169 (Area Clearance)
specifies the number of the subprogram that defines the perimeter of the
pocket. If you have defined shape #1 in CAM, and subprogram O1 does
not exist in the G-code program, then programming W1 in G169 will use
the shape defined in CAM. If subprogram O1 does exist in the G-code
program, then it will be used. Similarly, you can use CAM shapes in
G45, G65, G66, and M98. Any shape you can create in CAM, you can
use with this method in a G-code program.
Sample Programs
This chapter contains several programs that show typical uses for CNC
CAM programming. As a rule, blueprints having vague or limited data are
suitable for CAM Mode.
ANILAM suggests that you study this chapter and familiarize yourself with
the CAM Mode keystrokes.
Each example begins with a drawing, and proceeds through the
programming process from Create to Post. All keystrokes are detailed.
If working in metric, refer to the drawings for the appropriate dimensions.
It is assumed that you have already read and understood the materials in
this manual that pertain to CAM Programming.
Example #1 Machining an Outside Profile with Contour
X0 Y0 is set at the upper left corner of the part. Refer to Figure 18-7.
No construction geometry is required to create this shape. As you
program, note the prompts that appear each time you press ENTER.
3.0”
R = .75”
1.5”
1.5”
30 deg.
2.0”
5.5”
R = 1.5”
CAM1
Figure 18-7, An Outside Profile Using Contour
18-48
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Keystrokes:
1
F2 PROGRAM
2
F2 Create
3
Type CONTUR-1 press ENTER
4
F4 CAM
5
F3 S-EDIT
6
Create
7
ENTER
8
Cursor right, ENTER, 3 ENTER
9
Cursor down to #2 ENTER, -1.5 ENTER
10
Cursor up ENTER, 5 ENTER
11
F9 SETUP, Settings, ENTER (change to Incremental), F9 (to exit
window), F9 again.
12
Cursor down to #5 (Angle and X) ENTER, 1.5 ENTER, -30 ENTER
13
F9 SETUP, Settings, ENTER (switch back to Absolute), F9, F9
14
Cursor up to #2 ENTER, -5.5 ENTER
15
Cursor up ENTER, 0 ENTER
16
Cursor down to #2 ENTER, 0 ENTER
17
F5 ENTER (to Fit on screen)
18
F2 SHAPE
19
F4 six times (Back up to put in 1st radius)
20
Cursor left, then down to #4 (Rnd) ENTER, .75 ENTER
21
F5 four times (Forw, to next radius)
22
ENTER
23
F2 SHAPE (Off)
24
F5 ENTER (to Fit and redraw)
(to select the current Point definition), 0 ENTER, 0 ENTER
(to select Rnd), 1.5 ENTER
The shape is now ready for machining with one of the processes of the
MOTION (F7) key. Contour will be used for the example in Table 18-23,
Example 1 Settings: Contour Parameters with Outside Profile.
All rights reserved. Subject to change without notice.
17-April-04
18-49
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
25
F7 MOTION
26
Contour
27
Set parameters in the Contour Menu(s):
Table 18-23, Example 1 Settings: Contour Parameters with Outside Profile
Contour Parameters Menu 1 Values
Parameter
Shape number
Tool compensation
Tool diameter
XY stepover
Number of XY passes
Z step
Approach height
Top of contour
Bottom of contour
Stepover direction
More
Setting
1
CAM Left
0.7500
0.0000
1
0.0000
0.1000
0.0000
-0.3750
Toward
ENTER
Contour Parameters Menu 2 Values
Parameter
Comment
Interference check
Tool path color
Shape Reversed
Entry Move
Exit move
Machine setup
Setting
N/A
On
(Choose color)
No
N/A
N/A
ENTER
Contour Parameters Menu 3 Values
Parameter
Tool change
Initial move
Coolant at start
Coolant at end
Feedrate
Z Feedrate
Spindle at start
Spindle at end
Spindle speed
18-50
Setting
N/A
2D
On
Off
12.0
6.0
Forw
Off
1750
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
28
F10, F10
29
F8 Calc
30
F1 Yes
31
F4 View, choose Iso
32
F8 POST
33
F10 Exit (to Program Directory)
34
F5 List, to view G-code created, then F10 Exit.
After listing the G-code, go to Draw Graphics Mode (F7), and view the
program CAM Mode created. Press Load (F6) in the Program Directory
to load the program. Enter the tool offsets, zero setting, dry run(s), and
perform any other machine setup procedures now, before you produce
any parts.
All rights reserved. Subject to change without notice.
17-April-04
18-51
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Example #2 Machining a Slot using Contour
In Figure 18-8, X0 Y0 is set at the center of the large radius. CG is
required to create this shape. As you program, note the prompts that
appear each time you press ENTER.
R=1.25
R=.75
X5,Y0
X0,Y0
CAM3
Figure 18-8, Milling a Slot Using Contour
Keystrokes:
1
2
3
4
5
6
7
8
9
10
11
12
13
14
15
16
17
18
19
20
21
F2 PROGRAM (if necessary)
F2 Create
Type CONTUR-2 press ENTER
F4 CAM
F3 S-EDIT
Create
ENTER, -1.25 ENTER, 0 ENTER
Cursor to construction geometry, switch to Circles
Cursor right, then up to #2 (Rad, Center), ENTER
1.25 ENTER, ENTER, 0 ENTER, 0 ENTER
ENTER (Rad, Center) again
.75 ENTER, ENTER, 5 ENTER, 0 ENTER(F5 ENTER to Fit on screen)
Cursor down to #5 (line tangent to 2 circles), ENTER
1 ENTER, 2 ENTER, 1 ENTER
ENTER again
2 ENTER, 1 ENTER, 1 ENTER
Cursor left, then down to Chain (#6), ENTER
1 ENTER, 3 ENTER, 2 ENTER, 4 ENTER, 1 ENTER, F9
Cursor up to Arcs (#2), ensure direction is CW
Cursor right (to XY end, RAD), ENTER
-1.25 ENTER, 0 ENTER, 1.25 ENTER.
The shape is now completed. Press SETUP (F9), highlight Geometry,
press ENTER, and then switch ALL to Off. The CNC will turn off the
Construction Geometry and the screen will contain only the shape.
22
18-52
F5, ENTER (to Fit the Shape on the screen)
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
23
24
F7 MOTION
Contour
Refer to Table 18-24 to set the following parameters in the Contour
menu(s):
Table 18-24, Example 2 Settings: Milling a Slot Using Contour
Contour Parameters Menu 1 Values
Parameter
Setting
Shape number
1
Tool compensation
CAM Right
Tool diameter
0.7500
XY stepover
0.0000
Number of XY passes
1
Z step
0.0000
Approach height
0.1000
Top of contour
0.0000
Bottom of contour
-0.5000
Stepover direction
Toward
More
ENTER
Contour Parameters Menu 2 Values
Comment
N/A
Interference check
On
Tool path color
(Choose color)
Shape Reversed
No
Entry Move
N/A
Exit move
N/A
Machine setup
ENTER
Machine Setup
Tool change
N/A
Initial move
2D
Coolant at start
On
Coolant at end
Off
Feedrate
10.0
Z Feedrate
5.0
Spindle at start
Forw
Spindle at end
Off
Spindle speed
1850
All rights reserved. Subject to change without notice.
17-April-04
18-53
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Entry move:
Exit move:
CIRCULAR, Arc length = 180.0
Arc radius = .5000 (F10 to exit)
CIRCULAR, Arc length = 180.0
Arc radius = .5000 (F10 to exit)
26
F10, F10
27
F8 Calc
28
F1 Yes
29
F4 View, choose Iso
30
F8 POST
31
Exit (to Program Directory)
32
F5 List, to view G-code created, then F10.
After listing the G-code go to Draw Graphics Mode (F7), and view the
program CAM Mode created. Press Select (F6) in the Program Directory
to select the program. Enter the tool offsets, zero setting, dry run(s), and
perform any other machine setup procedures now, before you produce
any parts.
18-54
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Example #3 Machining an Outside Profile using Contour
In Figure 18-9, X0 Y0 is set at the center of the large radius. As you
program, note the prompts that appear each time you press ENTER.
R=2”
6.25”
R=4”
X0, Y0
3.75”
R=1.8”
CAM2
Figure 18-9, Machining an Outside Profile Using Contour
1
F2 PROGRAM (if necessary)
2
F2 Create
3
Type CONTUR-3 press ENTER
4
F4 CAM
5
Cursor down to CG, switch to circles
6
Cursor right, then up to #2, (Rad, Center) ENTER
7
4 ENTER, ENTER, 0 ENTER, 0 ENTER
8
ENTER
9
2 ENTER, ENTER, 0 ENTER, 4.25 ENTER (F5 ENTER to Fit on screen)
10
Cursor left, down to CG, switch to Lines
11
Cursor right, up to Y line, ENTER, -3.75 ENTER
12
F5 ENTER (To Fit on screen)
13
Cursor left, down to CG, switch to Points
14
Cursor right, down to #5 (intersection), ENTER
15
1 ENTER, 3 ENTER, 1 ENTER
16
ENTER
17
F2 SHAPE
18
F9 DelGeom, 3 ENTER
19
F2 SHAPE (off), F5 ENTER (to Fit on screen / redraw)
again
again (for intersection), then 1 ENTER, 3 ENTER, 2 ENTER
All rights reserved. Subject to change without notice.
17-April-04
18-55
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
20
Cursor left, up to CG, switch to Circles
21
Cursor right, up to #1 (Round), ENTER
22
1.8 ENTER, 4 ENTER, 5 ENTER, F5 ENTER (To fit)
The Construction Geometry necessary to drive the cursor to "build" the
shape now exists. The next step is to create the shape and chain. That
is, feed the cursor around the Construction Geometry.
23
F3 S-EDIT
24
Create
25
Cursor down to #6 (CG existing point), ENTER, 5 ENTER
26
Cursor left, then down to #6 (Chain), ENTER
27
-3 ENTER, 1 ENTER, 1 ENTER, 2 ENTER, 1 ENTER, 1 ENTER, 1 ENTER,
3 ENTER, 1 ENTER, F9
The shape now exists. Note that Construction Geometry circles are CW
by default. If no minus sign was given for -3, the arc would be in the
wrong direction, but RevArc (in S-EDIT) could correct it. To show this
function, as well as show "multiple chains", follow these steps:
A
F2 SHAPE
B
F8 four times (DelMove)
C
F2 SHAPE (Off)
D
F5 ENTER (to Fit)
E
ENTER
F
3 1 2 1 3 ENTER (The space between each element number is
necessary when giving more than one element while chaining.)
G
1 ENTER, 1 ENTER, 1 ENTER, 1 ENTER (selecting the intersections)
H
F9
I
F2 SHAPE
J
F4 Back .... until cursor is at end of bad arc (3 times)
K
F3 S-EDIT
L
RevArc
M
F2 SHAPE (Off)
N
F5 ENTER (Fit)
(Chain)
The shape is now correct!
28
29
F9 SETUP
Geometry, All Off, F9, F9
Assume that a .7500 radius must be placed in two positions, where the 2"
radius meets the 4" radius. To accomplish this:
18-56
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
A
F2 SHAPE
B
F5 Forw
C
Cursor up to #4 (Rnd), ENTER
D
.75 ENTER
E
F5 Forw
F
ENTER
G
Arrow up, ENTER (arrow up recalls last value entered)
H
F2 SHAPE (Off)
I
F5 ENTER (Fit / Redraw)
The shape is now complete. Activate the Contour window and set the
contouring parameters to create the path.
Refer to Table 18-25 to set the following parameters in the Contour
menu(s):
30
F5 (Fit)
31
F7 MOTION
32
Contour
Table 18-25, Example 3 Settings: Machining an Outside Profile Using Contour
Contour Parameters Menu 1 Values
Parameter
Shape number
Tool compensation
Tool diameter
XY stepover
Number of XY passes
Z step
Approach height
Top of contour
Bottom of contour
Stepover direction
More
Setting
1
CAM Left
0.5000
0.0150
2
0.0000
0.1000
0.0000
-0.2500
Toward
ENTER
Contour Parameters Menu 2 Values
Comment
N/A
Interference check
On
Tool path color
(Choose color)
Shape Reversed
No
Entry Move
N/A
All rights reserved. Subject to change without notice.
17-April-04
18-57
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Contour Parameters Menu 1 Values
Parameter
Setting
Exit move
Machine setup
Tool change
Initial move
Coolant at start
Coolant at end
Feedrate
Z Feedrate
Spindle at start
Spindle at end
Spindle speed
N/A
ENTER
Machine Setup
N/A
2D
On
Off
13.0
6.5
Forw
Off
2300
34
F10, F10
35
F8 Calc
36
F1 Yes
37
F5 Display, Window. Move window to lower-right corner, ENTER, to
see the two passes created in the path.
38
F5 ENTER (to Fit)
39
F4 View, choose Iso
40
F8 (POST)
41
Exit (to Program Directory)
42
F5 List, to view G-code created, then F10.
After you list the G-code, press Draw (F7), to view the CAM program.
Press Load (F6) in the Program Directory. Enter tool offsets and zero
setting and perform dry run(s) and any other machine setup procedures
now, before you produce any parts.
18-58
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Example #4 Machining a Contour with Many Unknown Intersections
The contour illustrated in Figure 18-10 consists wholly of tangent arcs.
The drawing shows the minimum number and types of dimensions
required to construct the part. Contour will be used to machine the
profile. X0 Y0 is set at the center of the large radius. As you program,
note the prompts that appear each time you press ENTER.
Figure 18-10, A Contour with Many Unknown Intersections
Keystrokes:
1
2
3
4
5
6
7
8
9
10
11
12
13
14
15
16
17
18
19
20
21
F2 PROGRAM (if necessary)
F2 Create
Type CONTUR-4 press ENTER
F4 CAM
Cursor down to CG, switch to Circles
Cursor right, then up to #2, (Rad, Center) ENTER
10 ENTER, ENTER, 0 ENTER, 0 ENTER
F5 ENTER (Fit)
ENTER again
3 ENTER, ENTER, 0 ENTER, 6 ENTER (F5 ENTER to Fit on screen)
Cursor up to #1 ENTER, 2 ENTER, 1 ENTER, 2 ENTER, 1 ENTER
ENTER again, 2 ENTER, 1 ENTER, 2 ENTER, 2 ENTER
F5 ENTER (Fit / Redraw)
F3 S-EDIT
Create
Cursor down to #5 (intersection) ENTER
3 ENTER 1 ENTER
Cursor left, then up 1 (to place on Chain - #6), ENTER
1 ENTER, 4 ENTER, -2 ENTER, 3 ENTER, 1 ENTER, F9
F9 SETUP, Geometry, All Off, F9, F9
F5 ENTER (Fit) (2 times)
All rights reserved. Subject to change without notice.
17-April-04
18-59
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
The Shape is now ready to contour.
22
23
F7 MOTION
Contour
Refer to Table 18-26 to set the following parameters in the Contour
Menu(s):
Table 18-26, Example 4: A Contour with Many Unknown Intersections
Contour Parameters Menu 1 Values
Parameter
Setting
Shape number
1
Tool compensation
CAM Left
Tool diameter
1.0200
XY stepover
0.1250
Number of XY passes
4
Z step
0.5000
Approach height
0.1000
Top of contour
0.0000
Bottom of contour
-.2000
Stepover direction
Toward
More
ENTER
Contour Parameters Menu 2 Values
Parameter
Setting
Comment
N/A
Interference check
On
Tool path color
(Choose color)
Shape Reversed
No
Entry Move
N/A
Exit move
N/A
Machine setup
ENTER
Machine Setup
Parameter
Setting
Tool change
N/A
Initial move
2D
Coolant at start
On
Coolant at end
Off
Feedrate
15.0
Z Feedrate
7.5
Spindle at start
Forw
Spindle at end
Off
Spindle speed
1200
18-60
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
25
F10, F10
26
F8 Calc
27
F1 Yes
28
F5 ENTER (to Fit)
29
F4 View, choose Iso
30
F8 (POST)
31
EXIT
32
F5 List, to view G-code created, then F10.
(to Program Directory)
After you list the G-code, go to Draw Mode (F7), and view the CAM
Mode program. Press Load (F6) in the Program Directory. Enter tool
offsets, zero setting and perform dry run(s), and any other machine setup
procedures now, before you produce any parts.
Example #5 Contour with Many Unknown Intersections - All Tangent Arcs
In Figure 18-11, Contour will be used to machine the profile. X0 Y0
is set at the center of the part. As you program, note the prompts that
appear each time you press ENTER.
Figure 18-11, Contour with Many Unknown Intersections - All Tangent Arcs
Keystrokes:
1
F2 PROGRAM (if necessary)
2
F2 Create
3
Type CONTUR-5 press ENTER
4
F4 CAM
5
Cursor down to CG, switch to circles
All rights reserved. Subject to change without notice.
17-April-04
18-61
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
6
Cursor right, then up to #2, (Rad, Center) ENTER
7
1.5 ENTER, ENTER, 0 ENTER, 0 ENTER
8
F5 ENTER(Fit)
9
ENTER
10
2 ENTER, ENTER, 0 ENTER, 0 ENTER(F5 ENTER to Fit on screen)
11
Cursor left, down to CG, switch to Lines
12
Cursor right, down to #4 (line thru point at angle), ENTER
13
45 ENTER, ENTER, 0 ENTER, 0 ENTER
14
Cursor down to #5 (line at distance from another line), ENTER,
3 ENTER, .5 ENTER
15
ENTER
16
F2 SHAPE, F9 DelGeom, 3 ENTER
17
Cursor up to #4 ENTER, 45+120 ENTER, ENTER, 0 ENTER, 0 ENTER
18
Cursor down to #5 ENTER, 3 ENTER, .5 ENTER
19
ENTER
20
F9 DELGeom, 3 ENTER
21
Repeat Steps 17 - 20, except use 45+240 for Step 17
22
F2 SHAPE (Off)
23
F5 ENTER (Fit)
again
again, 3 ENTER, -.5 ENTER
again, 3 ENTER, -.5 ENTER
The Geometry necessary to feed the cursor now exists. Next, create a
shape:
18-62
24
F3 S-EDIT
25
Create
26
ENTER,
27
Cursor left, then down to Chain (#6), ENTER
28
1 9 2 8 1 7 2 6 1 5 2 4 1 (Note space between each
element number), ENTER.
29
Now the CAM will prompt for intersections. Intersection #2 is
needed for each prompt. Press 2 ENTER for each prompt (total of
twelve times), then F9
30
Cursor up to #2 (Arcs)
31
Cursor right, ENTER, 1.5 ENTER, 0 ENTER, 1.5 ENTER
32
F9 SETUP, Geometry, All Off, F9, F9
33
F5 ENTER (Fit)
1.5 ENTER, 0 ENTER
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
The basic shape now exists. Use the Rnd icon to blend radii at the
corners and program.
34
35
36
37
38
39
40
SHAPE
Back twelve times, to reach 1st blend intersection
Cursor left, down to #4 (Rnd) ENTER, .25 ENTER
F5 Forw, ENTER(to select Rnd again), arrow up ENTER
Repeat Step 37 until all blends are complete (10 times)
F2 SHAPE (Off)
F5 ENTER (Fit)
The shape is now completed and ready to Contour.
41
42
43
F7 MOTION
Contour
Refer to Table 18-27. Set the following parameters in the Contour
menu(s):
Table 18-27, Example 5: Contour with Many Unknown Intersections - Tangent Arcs
Contour Parameters Menu 1 Values
Parameter
Setting
Shape number
1
Tool compensation
CAM Left
Tool diameter
0.4375
XY stepover
0.0000
Number of XY passes
1
Z step
0.0000
Approach height
0.1000
Top of contour
0.0000
Bottom of contour
-0.250
Stepover direction
Toward
More
Enter
Contour Parameters Menu 2 Values
Comment
N/A
Interference check
On
Tool path color
(Choose color)
Shape Reversed
Yes
Entry Move
N/A
Exit move
N/A
Machine setup
ENTER
Machine Setup
Tool change
N/A
Initial move
2D
Coolant at start
On
Coolant at end
Off
All rights reserved. Subject to change without notice.
17-April-04
18-63
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Feedrate
Z Feedrate
Spindle at start
Spindle at end
Spindle speed
44
45
46
47
48
49
50
51
11.5
5.8
Forw
Off
2200
F10, F10
F8 Calc
F1 Yes NOTE: Path direction is opposite of SHAPE direction.
F5 ENTER (to Fit)
F4 View, choose Iso
F8 (POST)
Exit (to Program Directory)
F5 List, to view G-code created, then F10.
After you list the G-code, go to Draw Mode (F7), and view the program
CAM created. Press Load (F6) in the Program Directory to load the
program. Enter tool offsets, zero setting and perform dry run(s), and any
other machine setup procedures now, before you produce any parts.
Example #6 Pocket Milled into Workpiece
Refer to Figure 18-7, An Outside Profile Using Contour. Pocket will be
used to machine the pocket. X0 Y0 is set at the upper left corner of the
pocket shape. No CG will be necessary. As you program, note the
prompts that appear each time you press ENTER.
Keystrokes:
1
2
3
4
F2 PROGRAM (if necessary)
F2 Create
Type POCKET-1 press ENTER
Refer to “Example #1.” Perform Steps 4 to 24, then continue with
Step 5 below.
The shape is now ready to be machined with the Pocket selection of the
F7 (MOTION) key.
5
6
7
18-64
F7 MOTION
Pocket
Refer to Table 18-28, Example 6 Settings: Pocket Milled into
Workpiece. Set the following parameters in the Pocket menu(s):
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Table 18-28, Example 6 Settings: Pocket Milled into Workpiece
Pocket Parameters Menu 1 Values
Parameter
Shape number
Tool diameter
XY stepover
XY Stock
Z step
Approach height
Top of pocket
Bottom of pocket
Island setup
More
Setting
1
0.7500
0.4000
0.0150
0.0000
0.1000
0.0000
-0.2500
Int
ENTER
Pocket Parameters Menu 2 Values
Parameter
Comment
Interference check
Angle of cut
Direction of cut
Start point
Tool path color
Shape Reversed
Entry Move
Exit move
Machine setup
Tool change
Initial move
Coolant at start
Coolant at end
Feedrate
Z Feedrate
Spindle at start
Spindle at end
Spindle speed
Setting
N/A
On
Default
Forw
Default
(Choose color)
No
N/A
N/A
ENTER
Pocket Parameters 3 Values
N/A
2D
On
Off
13.0
6.5
Forw
Off
1750
NOTE: No Z stock will be programmed in the pocket examples. If
required, Z stock can be programmed, then another "Pocket"
should be programmed to fit the bottom of the pocket.
All rights reserved. Subject to change without notice.
17-April-04
18-65
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
NOTE: All Pockets will require a "Contour" pass around the perimeter of
the pocket, to finish the sides (see “Example #1” to
“Example #5” for Contour). Therefore, ANILAM recommends
that XY stock be programmed for each Pocket.
8
9
10
F10, F10
F8 Calc
F2 No
NOTE: The lower area of the pocket is not completely cleared. This is
due to the XY stepover programmed in the first Pocket Menu.
To erase the path, select No when prompted to Save path?.
To change the stepover, press Calc again.
11
12
13
14
15
16
17
18
19
20
F7 MOTION
Pocket
Change XY stepover to .425
F8 Calc
F1 Yes
F5 ENTER (to Fit)
F4 View, choose Iso
F8 (POST)
Exit (to Program Directory)
F5 List, to view G-code created, then F10.
After you list the G-code, go to Draw Mode (F7), and view the program
CAM created. Press Load (F6) in the Program Directory to load the
program. Enter tool offsets, zero setting and perform dry run(s), and any
other machine setup procedures now, before you produce any parts.
18-66
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Example #7 Milled Pocket - X0 Y0 at Center of Radius
Refer to Figure 18-12. Pocket will be used to machine the pocket. X0
Y0 is set at the center of the radius. As you program, note the prompts
that appear each time you press ENTER.
R=2.0
6.0”
.50” TYP
CAM5
Figure 18-12, Milled Pocket - X0 Y0 at Center of Radius
Keystrokes:
1
2
3
4
5
6
7
8
9
10
11
12
13
14
F2 PROGRAM (if necessary)
F2 Create
Type POCKET-2, press ENTER
F4 CAM
Cursor down to CG, switch to Circles
Cursor right, then up to #2, (Rad, Center) ENTER
2 ENTER, ENTER, 0 ENTER, 0 ENTER
F5 ENTER (Fit)
Cursor left, then down to CG, switch to Lines
Cursor right, then up to Y line, ENTER
-4 ENTER
F5 ENTER (Fit)
Cursor down to #6 (line tangent to circle thru point) ENTER
1 ENTER, ENTER(to select current point def.) .5 ENTER, -4 ENTER, 2
ENTER
15
16
ENTER again
1 ENTER, ENTER, -.5 ENTER, -4 ENTER, 1 ENTER
All rights reserved. Subject to change without notice.
17-April-04
18-67
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
The geometry necessary to feed the cursor now exists.
17
F3 S-EDIT
18
Create
19
Cursor down to #5 (INTERSECTION), ENTER
20
2 ENTER, 4 ENTER
21
Cursor left, then down to Chain, ENTER
22
2 ENTER, 3 ENTER, -1 ENTER, 4 ENTER, 2 ENTER, F9
23
F9 SETUP, Geometry, All Off, F9, F9
24
F5 E ENTER (Fit)
The shape now exists and is ready to Pocket.
25
F7 MOTION
26
Pocket
27
Refer to Table 18-29. Set the following parameters in the
Pocket menu(s):
NOTE: With Z step set to .25 and Bottom of Pocket set to -.5000, two
depth-of-cuts will occur.
Table 18-29, Example 7: Pocket Parameters Menu 1 Values - X0 Y0 at Center of Radius
Pocket Parameters Menu 1 Values
Parameter
Setting
Shape number
1
Tool diameter
0.5000
XY stepover
0.3000
XY stock
0.0100
Z step
0.2500
Approach height
0.1000
Top of pocket
0.0000
Bottom of pocket
-0.5000
More
ENTER
Pocket Parameters Menu 2 Values
Parameter
Setting
Comment
N/A
Interference check
On
Angle of cut
Default
Direction of cut
Forw
Start point
Default
Tool path color
(choose color)
Shape Reversed
No
Entry Move
N/A
Exit move
N/A
Machine setup
ENTER
(Continued…)
18-68
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Table 18-29, Example 7: Pocket Parameters Menu 1 Values - X0 Y0 at Center of Radius
(Continued)
Pocket Parameters 3 Menu Values
Parameter
Setting
Tool change
N/A
Initial move
2D
Coolant at start
On
Coolant at end
Off
Feedrate
15.0
Z Feedrate
7.5
Spindle at start
Forw
Spindle at end
Off
Spindle speed
2550
28
29
30
31
32
33
34
35
F10, F10
F8 Calc
F1 Yes
F5 ENTER (to Fit)
F4 View, choose Iso
F8 (POST)
Exit (to Program Directory)
F5 List, to view G-code created, then F10.
After you list the G-code, go to Draw Mode (F7), and view the program
CAM created. Press Load (F6) in the Program Directory to load the
program. Enter tool offsets, zero setting and perform dry run(s), and any
other machine setup procedures now, before you produce any parts.
All rights reserved. Subject to change without notice.
17-April-04
18-69
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Example #8 Pocket Milled into Workpiece - X0 Y0 at Lower-Left Corner
Refer to Figure 18-13. Pocket will be used to machine the pocket. As
you program, note the prompts that appear each time you press ENTER.
2.50”
3.895
2.625”
R=.875
R=1.0”
2.506
R=1.0
1.50”
R=.25”
CAM6
Figure 18-13, Pocket Milled into Workpiece - X0 Y0 at Lower Left Corner
Keystrokes:
1
2
3
4
5
6
7
8
9
10
11
12
13
14
15
16
17
18
19
20
18-70
F2 PROGRAM (if necessary)
F2 Create
Type POCKET-3 press ENTER
F4 CAM
F3 S-EDIT
Create
ENTER (to select current point def), 0 ENTER, 0 ENTER
Cursor right, then down to Y line, ENTER
1.5 ENTER
Cursor left, then down to construction geometry, switch to Circles
Cursor right, then up to #2, ENTER, 1 ENTER, ENTER, 1 ENTER,
1.5 ENTER
ENTER again
.875 ENTER, ENTER, 2.5 ENTER, 2.625 ENTER
F5 ENTER (Fit)
ENTER again
1 ENTER, ENTER, 3.895 ENTER, 2.506 ENTER
Cursor down to #5 ENTER, 3 ENTER, 2 ENTER, 1 ENTER
Cursor up to #1 ENTER, .25 ENTER, 3 ENTER, 4 ENTER, 3 ENTER
F5 ENTER (Fit)
Cursor down to #6 ENTER, 270 ENTER, 5 ENTER, 2 ENTER
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
The necessary geometry now exists.
21
22
23
24
25
26
27
Cursor left, then down to Chain, ENTER
1 -2 4 -3 5 6 ENTER, F9 (Note spaces)
Cursor up to #1, Cursor right, then down to #2
ENTER, 0 ENTER
Cursor up to #1 ENTER, 0 ENTER
F9, Geometry, All Off, F9, F9
F5 ENTER (Fit)
The shape now displays in the graphics.
28
29
30
F7 MOTION
Pocket
Refer to Table 18-30. Set the following parameters in the Pocket
menu(s):
Table 18-30, Example 8 Settings: Pocket X0 Y0 at Lower Left Corner
Pocket Parameters Menu 1 Values
Parameter
Shape number
Tool diameter
XY stepover
XY stock
Z step
Approach height
Top of pocket
Bottom of pocket
More
Setting
1
0.3750
0.2000
0.0100
0.0000
0.1000
0.0000
-0.1875
ENTER
Pocket Parameters Menu 2 Values
Comment
N/A
Interference check
On
Angle of cut
Default
Direction of cut
Forw
Start point
Default
Tool path color
Yellow
Shape Reversed
No
Entry Move
N/A
Exit move
N/A
Machine setup
ENTER
(Continued…)
All rights reserved. Subject to change without notice.
17-April-04
18-71
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Table 18-30, Example 8 Settings: Pocket X0 Y0 at Lower Left Corner
(Continued)
Pocket Parameters 3
Parameter
Tool change
Initial move
Coolant at start
Coolant at end
Feedrate
Z Feedrate
Spindle at start
Spindle at end
Spindle speed
Setting
N/A
2D
On
Off
11.0
5.5
Forw
Off
2800
NOTE: All Pockets will require a "Contour" pass around the perimeter of
the pocket, to finish the sides (Refer to “Example #1” to
“Example #5” for Contour). Therefore, ANILAM recommends
that you program XY stock for each Pocket. You can also
program Z stock, which would require you to program a second
"Pocket" (with 0 Z stock) to finish the bottom.
NOTE: Set color to Yellow.
NOTE: No Entry/Exit moves will be used here.
31
32
33
34
35
36
37
38
F10, F10
F8 Calc
F1 Yes
F5 ENTER (to Fit)
F4 View, choose Iso
F8 (POST)
Exit (to Program Directory)
F5 List, to view G-code created, then F10.
After you list the G-code, go to Draw (F7), and view the program CAM
created. Press Load (F6) in the Program Directory to load the program.
Enter tool offsets, zero setting and perform dry run(s), and any other
machine setup procedures now, before you produce any parts.
18-72
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Example #9 Milled Pocket - X0 Y0 at the Center of the Large Radius
Pocket will be used to machine the pocket. The shape will be the same as
that used in “Example #2.” As you program, note the prompts that appear
each time you press ENTER.
Keystrokes:
1
F2 PROGRAM (if necessary)
2
F2 Create
3
Type CONTUR-2 press ENTER
4
F4 CAM
5
Refer to Table 18-31. Go to “Example #2,” and perform Steps 5
through 23, then continue with Step 6 below.
The Shape is now ready to be machined with the Pocket selection of the
MOTION (F7) key.
6
7
8
F7 MOTION
Pocket
Refer to Table 18-31. Set the following parameters in the Pocket
menu(s):
Table 18-31, Example 9 Settings: Pocket with X0 Y0 at the Center of the Large Radius
Pocket Parameters Menu 1 Values
Parameter
Setting
Shape number
1
Tool diameter
0.5000
XY stepover
0.2800
XY stock
0.0150
Z step
0.0000
Z stock
0.0000
Approach height
0.1000
Top of pocket
0.0000
Bottom of pocket
-0.1250
More
N/A
Pocket Parameters Menu 2 Values
Comment
N/A
Interference check
On
Angle of cut
60.00
Direction of cut
Forw
Start point
Default
Tool path color
(choose color)
Shape Reversed
No
Entry Move
N/A
Exit move
N/A
Machine setup
N/A
(Continued…)
All rights reserved. Subject to change without notice.
17-April-04
18-73
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Table 18-31, Example 9 Settings: Pocket with X0 Y0 at the Center of the Large Radius
(Continued)
Pocket Parameters 3
Parameter
Setting
Tool change
N/A
Initial move
2D
Coolant at start
On
Coolant at end
None
Feedrate
12.0
Z Feedrate
3.0
Spindle at start
Forw
Spindle at end
none
Spindle speed
2100
NOTE: All Pockets will require a "Contour" pass around the perimeter of
the pocket, to finish the sides (Refer to “Example #1” to
“Example #5” for Contour). Therefore, ANILAM recommends
that you program XY stock for each Pocket. You can also
program Z stock, which would require you to program a second
"Pocket" (with 0 Z stock) to finish the bottom.
NOTE: If default angle is set, pocket will not clear correctly because the
first move is an arc.
NOTE: No Entry/Exit moves will be used here.
8
9
10
11
12
13
14
15
F10, F10
F8 Calc
F1 Yes
F5 ENTER (to Fit)
F4 View, choose Iso
F8 (POST)
Exit (to Program Directory)
F5 List, to view G-code created, then F10.
After you list the G-code, go to Draw Mode (F7), and view the program
CAM created. Press Load (F6) in the Program Directory to load the
program. Enter tool offsets, zero setting and perform dry run(s), and any
other machine setup procedures now, before you produce any parts.
18-74
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Example #10 Series of Holes using Drill
Refer to Figure 18-14. No Construction Geometry will be used in this
example. X0 Y0 is set at the upper left corner of the part. As you
program, note the prompts that appear each time you press ENTER.
1.0”
3.0”
1.0”
1.75”
.250” Dia. (4)
CAM7
Figure 18-14, Series of Holes Using Drill
Keystrokes:
1
2
3
4
5
6
7
8
9
10
11
12
13
14
15
16
F2 PROGRAM (if necessary)
F2 Create
Type DRILL-1 press ENTER
F4 CAM
F3 S-EDIT
Create
ENTER (to select current point def), 1 ENTER, -1 ENTER
F9 SETUP, ENTER (to switch to Incremental), F9, F9
Cursor right, ENTER, 3 ENTER
Cursor down ENTER, -1.75 ENTER
Cursor up ENTER, -3 ENTER
F5 ENTER (Fit)
F5 (Half)
F7 MOTION
Drill
Refer to Table 18-32, Example 10 Settings: Series of Holes
Using Drill. Set the following parameters in the Drill menu(s):
All rights reserved. Subject to change without notice.
17-April-04
18-75
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Table 18-32, Example 10 Settings: Series of Holes Using Drill
Drill Parameters Menu 1 Values
Parameter
Setting
Shape number
1
Drill Cycle
Spot Drilling
Tool diameter
0.2500
Drill Parameters
ENTER
Tool path color
(choose color)
Machine setup
ENTER
G81 Spot Drilling Menu Values
Hole Depth
-.2250
Starting Height
0.1000
Return Height
0.1000
Drill Parameters 2 Menu Values
Tool change
N/A
Initial move
2D
Coolant at start
On
Coolant at end
Off
Feedrate
11.0
Spindle at start
Forw
Spindle at end
Off
Spindle speed
1800
17
18
19
20
21
22
23
F10
F8 Calc
F1 Yes
F4 View, choose Iso
F8 (POST)
Exit (to Program Directory)
F5 List, to view G-code created, then F10.
After you list the G-code, go to Draw Graphics Mode (F7), and view the
program CAM created. Press Load (F6) in the Program Directory to load
the program. Enter tool offsets, zero setting and perform dry run(s), and
any other machine setup procedures now, before you produce any parts.
Drilling will occur at the intersection of every move of the chosen shape.
If more than one hole size is required, program a shape for each hole
size.
Press ENTER with the cursor on "Drill Cycle" (Menu #1). All possible drill
cycles are displayed. Place the cursor on any one to select it, and press
ENTER. The CNC displays the appropriate drill parameters.
18-76
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Example #11 Pocket, Contour and Drill
Refer to Figure 18-15. Pocket will be used to rough-mill the pocket;
Contour will be used to finish the edges of the pocket; Drill will be used
to drill the holes into the bottom of the pocket. X0 Y0 is set at the upper
left corner of the part. As you program, note the prompts that appear
each time you press ENTER
1.0” TYP.
(25.4MM)
2.4” Typ.
(60.96MM)
1.0” TYP.
(25.4MM)
1.2”
TYP.
(30.48MM)
Tool Rad.
O.K.
1.0” TYP.
(25.4MM)
3.0”
TYP.
(76.2MM)
EP
DE
5“ MM)
7
.18 .763
(4
1.0” TYP.
(25.4MM)
1.5” TYP.
(38.1MM)
CAM8
Figure 18-15, Rough-Milled Pocket Using Pocket, Contour and Drill
Plan to use the following tools:
Tool #1 = 1/2" end mill.
Tool #2 = 3/8" drill.
Keystrokes:
1
2
3
4
5
6
7
8
9
10
11
12
13
14
F2 PROGRAM (if necessary)
F2 Create
Type ALL-1 press ENTER
F4 CAM
F3 S-EDIT
Create
ENTER (to select current point def), 1 ENTER, -1 ENTER
F9 SETUP, Settings, ENTER (to switch to Incremental), F9, F9
Cursor right, ENTER, 2.4 ENTER
Cursor down two, ENTER, 1.2 ENTER, -1 ENTER
Cursor up two ENTER, 2.4 ENTER
Cursor down ENTER, -3 ENTER
Cursor up ENTER, -2.4 ENTER
Cursor down two ENTER, -1.2 ENTER, 1 ENTER
All rights reserved. Subject to change without notice.
17-April-04
18-77
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
15
16
Cursor up two ENTER, -2.4 ENTER
Cursor down ENTER, 3 ENTER
The pocket (and contour) shape now exists.
17
18
19
20
21
F3 S-EDIT
Create
ENTER (to select current point def), 2 ENTER, -2.5 ENTER
Cursor down ENTER, 4 ENTER, -1 ENTER
A (for Autofit)
The drill shape now exists.
22
23
24
F7 Motion
Pocket
Refer to Table 18-33. Set the following parameters in the Pocket
Menu(s):
Table 18-33, Example 11: Pocket Parameters Menu Values - Pocket, Contour and Drill
Pocket Parameters Menu 1 Values
Parameter
Shape number
Tool diameter
XY stepover
XY stock
Z step
Approach height
Top of pocket
Bottom of pocket
More
Setting
1
0.5000
0.1700
0.0150
0.0000
0.1000
0.0000
-0.1875
ENTER
Pocket Parameters Menu 2 Values
Comment
N/A
Interference check
On
Angle of cut
Default
Direction of cut
Forw
Start point
Default
Tool path color
(choose color)
Shape Reversed
No
Entry Move
N/A
Exit move
N/A
Machine setup
ENTER
(Continued…)
18-78
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Table 18-33, Example 11: Pocket Parameters Menu Values - Pocket, Contour and Drill
(Continued)
Pocket Parameters Menu 3 Values
Parameter
Tool change
Initial move
Coolant at start
Coolant at end
Feedrate
Z Feedrate
Spindle at start
Spindle at end
Spindle speed
Setting
N/A
2D
On
None
12.0
3.0
Forw
None
2100
25
26
27
28
29
F10, F10
F8 Calc
F1 Yes
F7 MOTION
Contour
30
Refer to Table 18-34. Set the following parameters in the Contour
menu(s):
Table 18-34, Example 11: Contour Parameters Menu Values - Pocket, Contour and Drill
Contour Parameters Menu 1 Values
Parameter
Setting
Shape number
1
Tool compensation
CAM Left
Tool diameter
0.5000
XY stepover
0.0150
Number of XY passes
2
Z step
0.0000
Approach height
0.1000
Top of contour
0.0000
Bottom of contour
-0.1875
Stepover direction
Toward
More
ENTER
Contour Parameters 2 Menu Values
Comment
N/A
Interference check
On
Tool path color
Yellow
Shape Reversed
Yes
Entry Move
N/A
Exit Move
N/A
Machine setup
ENTER
(Continued…)
All rights reserved. Subject to change without notice.
17-April-04
18-79
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Table 18-34, Example 11: Contour Parameters Menu Values - Pocket, Contour and Drill
(Continued)
Contour Parameters 3
Parameter
Setting
Tool change
N/A
Initial move
2D
Coolant at start
None
Coolant at end
Off
Feedrate
10.0
Z Feedrate
10.0
Spindle at start
None
Spindle at end
Off
Spindle speed
0
NOTE: All Pockets will require a Contour pass around the perimeter of
the pocket, to finish the sides (Refer to “Example #1” to
“Example #5” for Contour). Therefore, ANILAM recommends
that you program XY stock for each Pocket. You can also
program Z stock, which would require you to program a second
"Pocket" (with 0 Z stock) to finish the bottom.
NOTE: Entry move; Set to: Type = LINEAR, Origin = 1.5, -1.5
Exit move; None used here. (F10 to exit).
31
32
33
34
35
36
F10, F10
F8 Calc
F1 Yes
F7 MOTION
Drill
Refer to Table 18-35. Set the following parameters in the Drill
menu(s):
Table 18-35, Drill Parameters Menu Values - Pocket, Contour and Drill
Drill Parameters 1 Menu Values
Parameter
Setting
Shape number
2
Drill Cycle
Peck Drilling
Tool diameter
0.3750
Drill Parameters
N/A
Tool path color
Red
Machine setup
ENTER
G83 – Peck Drilling Menu Values
Hole Depth
-.6500
Start Height
-.0875
Maximum Peck
0.1500
Return Height
0.1000
(Continued…)
18-80
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Table 18-35, Drill Parameters Menu Values - Pocket, Contour and Drill
(Continued)
Drill Parameters 2 Menu Values
Parameter
Setting
Tool Change
N/A
Initial move
2D
Coolant at start
On
Coolant at end
Off
Feedrate
9.5
Spindle at start
Fwd
Spindle at end
Off
Spindle speed
1200
37
38
39
40
41
42
43
44
F10
F8 Calc
F1 Yes
F4 View, choose Iso
ALT-A
F8 (POST)
Exit (to Program Directory)
F5 List, to view G-code created, then F10.
After you list the G-code, go to Draw Mode (F7), and view the program
CAM created. Press Load (F6) in the Program Directory to load the
program. Enter tool offsets, zero setting and perform dry run(s), and any
other machine setup procedures now, before you produce any parts.
All rights reserved. Subject to change without notice.
17-April-04
18-81
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Example #12 Using CAM for Pockets with Islands (G162)
Using CAM, the geometer would be entered as normal, with the island
inside the main profile. The pocketing and contours would be done the
same as any other CAM program.
The CAM display shows a shape with four islands in it with islands inside
of islands. The shape is already done. See Figure 18-16.
Figure 18-16, CAM Workpiece Illustration
1. Press Motion (F7).
2. Select Pocket.
3. Select Island setup (see Table 18-7, Pocket Parameters 1
Menu), and press ENTER to process islands.
4. Select Yes. The CNC asks which islands to process.
5. A pop-up menu is displayed with options: No, Ext, and Int.
No
Process island
Ext (external)
Island is cut around the outside
Int (internal)
Island is cut on the inside
Refer to Figure 18-17, CAM Workpiece Illustration with Pocket
Parameters.
18-82
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Figure 18-17, CAM Illustration with Pocket Parameters Pop-up Menu
After all islands are setup, press Calc. This clears the pocket, leaving
islands standing and cutting inserts in the islands.
The islands still have to be contoured as shown in figure below. See
Figure 18-18.
Figure 18-18, CAM Illustration with Contours
The CAM program is now ready to post and generate machine program.
Figure 18-19, CAM Pockets with Islands Illustration in Draw Mode shows
the CAM program in Draw mode.
All rights reserved. Subject to change without notice.
17-April-04
18-83
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Figure 18-19, CAM Pockets with Islands Illustration in Draw Mode
18-84
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - CAM Programming
Additional Drawings for Practice
Use Figure 18-20 and Figure 18-20 to improve your CAM programming
skills:
R 1”
R 4.5”
45 Deg.
Typ.
R 4”
R 5”
CAM9
Figure 18-20, Practice Drawing A
.441” TYP.
1.19”
R .19 (2)
45 deg.
R .031”
(2)
FULL
RAD.
3.97”
R .19”
3.601”
R 3.59”
3.31”
2.31”
2.62”
.562”
40 Deg.
.562”
R .81
Figure 18-21, Practice Drawing B
All rights reserved. Subject to change without notice.
17-April-04
18-85
CNC Programming and Operations Manual
P/N 70000487G - Advanced Programming Features
Section 19 - Advanced Programming Features
Modifiers
Use modifiers to alter the way the CNC interprets a word address. For
example, a single value in an Inch Mode program may be forced to Metric
Mode, without programming G71. Or, arc center values (I, J, or K) may
be forced to an absolute value.
The address and modifier must be accompanied by an ampersand (&).
Place the ampersand (&) between the address word to be modified and
the modifier. The address word is programmed first, followed by &,
followed by the modifier, followed by the value.
The modifier is non-modal and is applied only to the address word it
accompanies.
Example
G02 X2.0 Y1.0 I&A1.5 J&A1.0
The example forces the I and J center of an arc to be in Absolute Mode.
I and J are incremental by default. Assume the axes are at X1 Y1.
Table 19-1 lists the available modifiers.
Table 19-1, Modifiers
Force the address word to be in Absolute Mode.
Force the address word to be in Incremental Mode.
Force the address word to be in Inch Mode.
Force the address word to be in Millimeter Mode.
Force the address word to be an absolute metric position
from Machine Home. All offsets (G53, G92, TLO) are
ignored.
A
D
E
M
P
Block Separators
Block separators (;) can be used to place several functions on one line of
a program. This is useful in Manual Data Input (MDI) Mode because you
can combine several commands on one line at the command line.
Example 1 will execute five moves on the machine when you press
START. Each move is separated by the (;) block separator.
Example 1:
G90 G01 X0 Y0 F30 ; X3 ; Y-2 ; X0 ; Y0
Example 2 will move the axes linearly to X0 Y0, then CW to X1 Y1, then
linearly to X2.
All rights reserved. Subject to change without notice.
17-April-04
19-1
CNC Programming and Operations Manual
P/N 70000487G - Advanced Programming Features
Example 2:
G90 G01 X0 Y0 F10 ; G02 X1 Y1 I1 J0 F8 ; G01 X2
In MDI Mode, you can type up to two lines of text at the command line.
This makes it possible to program a number of sequential moves without
beginning a new line of text.
The MDI command line will wrap around when the first line is filled,
bringing the cursor down one line. When the second line is full, the limit
has been reached.
The number of separate steps in a program file is limited only by the
available memory.
Block separators can also be used in programs.
Tool Offset Modification
You can modify a tool diameter or length offset in the program without
using the Tool Page. This is useful when rough-milling a profile where
cutter diameter compensation requires different diameter definitions for
the same tool to step the width of the cut. Tool modification can be either
temporary or permanent. To make it temporary, choose not to update
the Tool Page. To make it permanent, choose to update the Tool Page.
Refer to Figure 19-1.
X0, Y0
TOOLMOD
Figure 19-1, Tool Modification Programming Example
Temporary Format:
T1 D.5500 L-1.1000
Changes Tool 1 diameter offset to .5500 and length offset to -1.1000. Do
not update the Tool Page for Tool 1.
19-2
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Advanced Programming Features
Permanent Format:
T1 D.5500 L-1.1000 H
Changes Tool 1 diameter offset to .5500 and length offset to -1.1000.
Updates the Tool Page for Tool 1 to entered values.
D and L values are absolute and replace the previous offsets. They are
not added to existing offsets. The H command instructs the CNC to
update the Tool Page offsets to the programmed values.
Tool Modification Programming Example
This program will mill the square shape four times. The CNC executes
the first pass using the tool diameter entered in the Tool Page. Each
subsequent pass will use a different, “modified” tool diameter, as
programmed in Blocks 8, 10, and 12. T, D, L, and H are the only word
addresses allowed on the block.
N1
N2
N3
N4
N5
N6
N7
N8
N9
N10
N11
N12
N13
N14
N15
N16
N17
N18
N19
N20
N21
N22
N23
N24
N25
N26
N27
All rights reserved. Subject to change without notice.
17-April-04
O41 * TOOL-MOD.G
G90 G70 G0 G17
T0
Z0
X0 Y0
T1 * .8000 DIA.
M98 P1
T1 D.6
M98 P1
T1 D.4
M98 P1
T1 D.2
M98 P1
T0
G0 Z0
M2
O1 * SUBPGM-1
G1 Z-.25 F10
G41 Y1
X-1
Y-1
X1
Y1
X0
G40 Y0
M99
19-3
CNC Programming and Operations Manual
P/N 70000487G - Advanced Programming Features
The main program calls the subprogram that contains the compensation
on/off commands between each tool modification.
NOTE: When tool modifiers are activated, the CNC still applies any
wear offset entered in the Tool Page.
Expressions and Functions
You can program some values as expressions. Parentheses enclose
expressions. The CNC displays an error message if the expression is
incorrectly entered. Expressions follow the standard mathematics order
of operations (multiplication, division, addition and subtraction).
An expression must contain an operator or use a function. Refer to
Table 19-2.
Table 19-2, Operators and Functions
Ref.
a)
b)
c)
d)
e)
f)
g)
h)
i)
j)
k)
l)
m)
n)
o)
p)
q)
r)
s)
t)
u)
v)
w)
x)
y)
z)
19-4
Expression
()
*/&
+><
= !=
tomm
toin
tode
tonu
round
fix
fup
var
sin
cos
tan
asin
acos
atan
abs
sqrt
ln
log
exp
trun
!+-#
Function
Expression function (parenthesis)
Multiplication, division, modification
Addition, subtraction
Relation greater than, less than
Relation equal, not equal
Convert to mm
Convert to inch
Convert to inch if inch, mm if mm
Force to current modal
Round up or down, automatically
Discard fraction less than 1
Raise fraction 1
True if defined, false otherwise
Sine
Cosine
Tangent
Arcsine
Arcosine
Arctangent
Absolute value
Square root
Natural logarithm
Logarithm
Exponential
Truncate
Unary logical not, positive, negative,
indirection
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Advanced Programming Features
Examples
Ref. from
Previous
Table
a)
b)
c)
d)
e)
f)
g)
h)
i)
j)
k)
l)
m)
n)
o)
p)
q)
r)
s)
t)
u)
v)
w)
x)
Example
G01 X(#100 + #101). All calculations must be enclosed in
parentheses. This defines an expression.
G00 Y&A(#102 * #103)
LOOP (5 / 2 / .01)
Example of multiplication, division and modification.
G01 X(3 + 2)
#100 = (#122 - #105).
Addition and Subtraction.
IF (#101 > 0) THEN ....
Greater than (>), less than (<).
IF (#144 = #143) GOTO .....
Equal to, not equal to (!=).
TOMM (n); convert n to mm.
If n's type is inch, TOMM (n) = n * 25.4.
TOIN (n); convert n to inch. If n's type is mm, TOIN (n) = n
/ 25.4.
TODE (n); convert to current (IN or MM) mode.
TONU (n); force the type of (n) to the modal (inch or mm).
ROUND (n) will round the value of (n) up or down,
depending if its fractional part is equal or greater than
0.500000, or less than 0.500000.
#100 = 1.500 ; G01 X(round(#100)) will move to X2.0000
#101 = 1.499 ; G01 X(round(#101)) will move to X1.0000
FIX (n) will round the value down to the next whole
number. #100 = (5/2) ; G01 X(fix(#100)) will move to
X2.0000
FUP (n) will round the value up to the next whole number.
#100 = (5/2) ; G01 X(fup(#100)) will move to X3.0000
VAR (n) is used to check if a user variable has been
defined in a program. IF (var(#100)) THEN .... If #100 has
been defined by the user, then true. If not, then false.
SIN (n) will give the sine of (n). (n) is assumed to be in
degrees. G01 X(cos(15)) Y(sin(15)) will move along the
hypotenuse of a 15-degree angle with a hypotenuse of 1.
COS (n) will give the cosine of (n).
TAN (n) will give the tangent of (n).
ASIN (n) will give the arcsine of (n).
ACOS (n) will give the arccosine of (n).
ATAN (n) will give the arctangent of (n).
ABS (n) will give the absolute value of (n).
SQRT (n) will give the square root of (n).
LN (n) is natural logarithm.
LOG (n) is logarithm.
EXP (n) is exponential function.
All rights reserved. Subject to change without notice.
17-April-04
19-5
CNC Programming and Operations Manual
P/N 70000487G - Advanced Programming Features
Ref. from
Previous
Table
y)
z)
Example
TRUN (n) will truncate the value of (n).
! unary logical not, != (not equal to) ; positive, (+(#100))
means positive whatever value is in #100 ; negative, ((#100)) means negative whatever is in #100 ; indirection.
Example of indirection:
N30 #200 = 51.456
N40 #201 = 200
N50 G90 G1 X ##201 F200
At Block N40 variable #201 = 200. Only when the second
level of indirection is used at N50 does variable #201
contain the contents of variable #200 causing the X-axis to
move to position 51.456. Up to four levels of indirection
can be used.
System Variables
Certain variables are set aside as CNC system variables. Some may be
useful for you to know when programming macros. The system variables
range from #1000 to #1099. Most of these variables are "read only".
You cannot write information to them. There are a few exceptions to this
rule. Refer to Table 19-3 for a list of available system variables. Table 19-3, System Variables
Variable
#1000 to #1009
#1010 to #1015
#1016
#1017
#1020
#1021
#1022
#1023
#1024
#1030
#1031
#1032
#1040
#1041
#1050 to #1055
19-6
Description
Block skip variables (read/write).
Commanded ABS tool position (x,y,z,u,v,w)
Current G motion mode (0=rapid, 1=feed,
2=cw arc, 3=ccw arc, 5=ellipse, 6=spiral).
Current XYZ plane (17=XY, 18=XZ, 19=YZ).
Current tool diameter.
Current tool length offset.
Current feedrate.
Current rapidrate.
Current RPM.
Stock variable (R/W).
Acute angle for rounding compensated
intersections (default = 15.0).
# of look-ahead blocks for cutter comp
(R/W).
Real-time tool compensation for ellipses and
spirals. 0=off, 1=outside, 2=inside.
Current program tool compensation (40=off,
41=left, 42=right).
Actual absolute position (X,Y,Z,U,V,W).
(Continued…)
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Advanced Programming Features
Table 19-3, System Variables (Continued)
Variable
#1070
#1071
#1090
#1091
#1099
Description
Current XYZ dimension (70=inch, 71=mm).
Current UVW dimension (70=inch, 71=mm).
Current XYZ dimension (90=abs, 91=incr).
Current UVW dimension (90=abs, 91=incr).
Last programmed Gear Range.
User Variables
Certain variables are set aside for the programmer to use. These may be
useful when programming macros. You can read from or write to these
variables. They are divided into four categories:
q
Local variables: #1 to #99
These variable numbers can be used only within the body of a
subprogram (or macro). The CNC generates an error message if you
program these variables in the main program. Values do not hold
from one subprogram to another. In this way, the same variables can
be used in separate subprograms, with different values.
q
Common (global) variables: #100 to #220. (Read/Write)
These variables can be used anywhere in the program or subprogram
and their value will remain.
q
Read only variables: #221 to #250
These variables can only be set in the main program. Once set, the
variables can be used in subprograms or macros as "read only"
variables.
q
Static (global) variables: #260 to #279. (Read/Write)
These variables can be used anywhere in the program or subprogram
and their value will remain across shutdowns or software resets.
WARNING: OEM and machine tool builders should use
#100–#150 and #260–#269 for any custom macros.
End users should use #151–#220 and #270–#279 for
your custom macros. This avoids conflicting usage
of the global variables.
Block skip variables: #1000 to #1009 (Refer to “Block Separators” in
this section.)
Variable Programming (Parametric Programming)
q
Variable, or parametric, programming enables you to create macros to
generate geometric shapes that are not already available in a canned
cycle.
Conditional loops, jumps, and GOTO commands can be used to control
program execution.
All rights reserved. Subject to change without notice.
17-April-04
19-7
CNC Programming and Operations Manual
P/N 70000487G - Advanced Programming Features
Parameters and Variable Registers
A macro is a series of instructions designed to achieve a specific result
for a given set of constraints. For example, a rectangular pocket of any
size always has four sides, four corner radii and a depth. Therefore, you
can cut many pockets of different sizes using a similar tool path with
longer or shorter moves for the tool path. If a suitable program
processes the constraints of the pocket, the CNC calculates a tool path to
cut a particular pocket. Such a program is called a macro. The G78
rectangular pocket cycle is an example of a macro that cannot be edited.
The constraints of the pocket, or the feature required, are its parameters.
Parameters for any feature will vary as dimensions change, therefore the
parameters are often called variables. The data for each parameter must
be stored as an entity, known as a variable register, also called variables.
Parameters passed to a macro will be called parameters in this manual.
Contents of Variables (PRINT)
Format:
PRINT xxx(variable)
Format:
N(Block number) PRINT xxx(variable)
You can verify the contents of a variable. This is useful when you are
debugging a program. Use the PRINT command to display the contents
of a variable on the CRT in Manual, Single-Step and Auto Modes.
Example 1:
PRINT 200
Displays the contents of the variable (#200).
Example 2:
N180 PRINT 110
To display variable contents during program execution, use the PRINT
command as part of the program. Example 2 will print the contents of
variables #110 to the CRT.
If commas separate the numbers, several variables can be printed
simultaneously.
In Manual Mode, type PRINT 110 then press START to display the
contents on the CRT.
The PRINT variable can be abbreviated, as follows: ]P
In the Editor, press Expand (F7) to expand the first character of print into
the full address. (Type P, then press F7). Refer to “Short Form
Addressing” in this section.
19-8
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Advanced Programming Features
Setting and Transferring Variables
When using parametric programming with axis addresses and
expressions (including unary minus), the complete expression needs to
be in parenthesis. For example, X(-#151) is correct. X-#151 or X-(#151)
are not correct.
Setting and Direct Transfer:
Variables are loaded or set when they appear on the left side of an
equation. (That is, the left side of the equal sign.)
Example 1:
N200 #100 = 5.56
Variable #100 contains number 5.560000 until changed.
Example 2:
N200 #100 = 25.4m
Variable #100 sets variable 100 to 25.4mm. Similarly, #100 = 5i sets
variable 100 to 5 inches. If neither “i” nor “m” are used when assigning a
variable, then the value of the variable is modal. For example, #100 = 8
sets variable #100 to 8 (no unit).
Example 3:
N200 #100 = #20
Variable #100 contains the number held by #20 until changed. Equating
one variable with another is called a direct transfer.
NOTE: When a direct transfer is requested, the variable on the right
side of the equation must contain a value. Otherwise, the CNC
displays an error message(#nn not defined).
Indirect Transfer:
You can indirectly transfer variables to a depth of four levels by
introducing extra hatch marks (#) before the variable number. In an
indirect transfer, a value is transferred to one variable via another.
Example 1:
N201
N202
N203
N204
G90 G17 G71 G0
#101 = 51.456
#102 = 101
X##102
At Block N204, the X-axis moves to 51.456. Example 1 shows single
indirection. The contents of variable #101 are used by variable #102.
The actual content of variable #102 is constant 101. The indirection is
activated at Block N204 by the addition of the (#) symbol to variable
#102.
All rights reserved. Subject to change without notice.
17-April-04
19-9
CNC Programming and Operations Manual
P/N 70000487G - Advanced Programming Features
Example 2:
N210
N211
N212
N213
N214
N215
N216
N217
N218
N219
N220
N221
G90 G17 G71 G0
#101 = 1
#102 = 2
#103 = 3
#104 = 4
#119 = 100
LOOP 4
#119 = #119 + 1
#120 = 119
X###120
END
M2
Example 2 contains two levels of indirection (N219) and shows how the
contents from multiple variables can be assigned to a command or
expression.
At Block N215, variable #119 is set to constant 100.
At Block N217 one is added to the contents of variable #119.
At Block N218 variable #120 is set to constant 119.
Block N219 moves the X-axis to the position contained in variable #120
via two levels of indirection. The first level is the content of variable #119.
The second level is the content of variable #101, which is incremented in
the loop at Block N217 to introduce the contents of variables #102, #103
and #104.
The X-axis will move to X1; X2; X3; and X4.
Storing Result of Computation
When a mathematical expression is programmed, variables on the left
side of an equation store the computed result.
N250 #110 = #20 + #35
N260 #120 = #18 / 2
At N250, #110 contains the sum of the contents of #20 and #35. At
N260, #120 contains the result of the contents of #18 divided by 2.
Parentheses establish an order of operations or denote special functions.
NOTE: Multiplication operations MUST be in parentheses or the CNC
treats the multiply command (*) as a comment sign and
disregards the rest of the line following the sign (*).
N300 #140 = (#11 * #115) / 2
N310 #141 = sin (45)
N320 #142 = (#141 * #140) ; * #142 is shortest side
19-10
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Advanced Programming Features
Variable Programming
Example 1
This program uses common variables in the range of #50 to #149. The
program mills a pocket with a three-degree draft angle on the sidewalls.
The dimensions at the bottom of the pocket are:
15.5730 (X axis) x 13.8850 (Y axis). The pocket is 1.0000 in. deep.
The tool begins at the upper-left corner of the pocket and at full depth.
Part Zero is set in the center of the pocket.
O 28 * 3-DEG. DRFT PKT
G90 G70 G0 G17
T0
Z0
X0 Y0
T1
X-7.7865 Y6.9425
Z.5
G1 Z-1 F10
F40
#101 = 15.5730
#102 = 13.8850
#103 = .0200
#104 = (#103*TAN(3))
M98 P100
T0
G90 G0 Z0
X0 Y0
M2
O100
LOOP((1/#103)+1);
G91
G1 Y(-#102);
X#101;
Y#102;
X(-#101);
X(-#104) Y#104 Z#103;
#101 = #101 + (#104*2);
#102 = #102 + (#104*2);
END
M99
All rights reserved. Subject to change without notice.
17-April-04
* MOVE TO UP-LEFT CORNER
* FEED TO DEPTH
* LENGTH (X) OF POCKET
* WIDTH OF POCKET
* DESIRED "STEP-UP" IN Z AXIS
* CALCULATE "STEP-OVER" IN X-Y AXES
* CALL SUBPROGRAM 100
* SET LOOP NUMBER (1 IN. DP / .02 STEP) + 1
* SET INCREMENTAL MODAL
* MILL L.H. SIDE
* MILL BOTTOM SIDE
* MILL R.H. SIDE
* MILL TOP SIDE, BACK TO START POS'N
* STEP UP/OVER IN X-Y AND Z
* ADD STEPOVER TIMES 2 TO LONG SIDES
* ADD STEPOVER TIMES 2 TO SHORT SIDES
* END LOOP
19-11
CNC Programming and Operations Manual
P/N 70000487G - Advanced Programming Features
The pocket will be milled with a side draft angle of three degrees. Z is set
to a step-up increment of .02 in. #152 can be set to a desired value,
perhaps to determine the finish on the sidewalls of the pocket. In this
example, the pocket will always have a depth of 1 in., and a draft angle of
3 degrees. The side lengths and Z step may be changed.
To make this program totally independent, the Z depth and draft angle
can be set to variables, and the additional calculations must then be
made.
Example 2
This program requires the length and width of a rectangle, the cut per
side on the rectangle, and the number of passes around the rectangle.
Variables #150 to #199 are read only. They can be set only in the main
program.
N10
N20
N30
N40
N50
N60
N70
N80
N90
N100
N110
N120
N130
N140
O 1000
G0 G17 G70 G90 F80
T0
Z0
X0 Y0 ;* START POSITION OF RECTANGLE
#151 = 3 ;* SET READ ONLY VARIABLE, X LENGTH OF SIDE
#152 = 3;* SET READ ONLY VARIABLE, Y LENGTH OF SIDE
#153 = .25 ;* SET READ ONLY VARIABLE, CUT PER SIDE
#154 = 5 ;* SET READ ONLY VARIABLE, NUMBER OF PASSES
M98 P1 ;* CALL SUBPROGRAM BODY
T0
Z0
X0 Y0
M2
N160
N170
N180
N190
N200
N210
N220
N230
N240
N250
N260
N270
N280
N290
N300
N310
N320
O1
G91 G1 X#151 ;* MOVE X AXIS LENGTH OF SIDE
Y#152 ;* MOVE Y AXIS LENGTH OF SIDE
X(-#151) ;* MOVE X NEGATIVE
Y(-#152) ;* MOVE Y NEGATIVE
#111 = 0 ;* SET SIDE CUT INCREMENT TO 0
LOOP #154 ;* LOOP #154 NUMBER OF TIMES
X#153 Y#153 ;* SET SIDE CUT
#111 = #111 - #153 ;* DECREMENT SIDE CUT EACH LOOP
#101 = #151 + (#111 * 2 ) ;* CALCULATE NEW X LENGTH
#102 = #152 + (#111 * 2 ) ;* CALCULATE NEW Y LENGTH
X#101 ;* MOVE AROUND SQUARE USING NEW SIDE * LENGTHS
Y#102
X(-#101)
Y(-#102)
END
M99
The read only variables are set in Blocks N60 to N90. Then, the
subprogram is called. At Block N170, the first move is made along the Xaxis, followed by a move along the Y-axis. At Blocks N190 and N200, the
19-12
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Advanced Programming Features
logical negative sign makes the axis move in the opposite direction. The
contents of the variables remain the same.
At Block N220, a loop, which ends at Block N310, is set up. The loop
runs the number of times contained in variable #154. The first move in
the loop is in the X and Y axes to the side of cut value in #153. In Block
N240, #111 decrements at each pass through the loop, by the value of
the side cut. This value, in turn, is used to calculate a new length of cut
for each side.
User Macros (G65, G66, G67)
Use G66 when you want to use a modal macro subprogram. These
groups of instructions can be special canned cycles made up by the user
to simplify the programming of the particular part, or master programs for
similar part families, programmed with variables rather than fixed
dimensions.
Macros can contain automatic measuring sequences for sensors, such as
a probe, for feedback to the CNC. Refer to Table 19-4.
Table 19-4, Macro G-Codes
Format
G65 Pn Ln
G66 Pn
G67
Macro Body Structure
Function
Non-modal macro call. Call macro n. Execute
macro, at the current position, only once. The
subprogram can be looped (L).
Modal macro call. Call macro n. Execute macro
at any X and/or Y location given after the G66
code, until G67 (cancel) is called. G66 will stay
active until G67 is called.
Cancel Modal Macro Call (G66).
The macro body is defined in the same way as a subprogram.
Format: Oxxx
O identifies it as a macro.
xxx is the label number.
Example:
N200 O 201
N210 -----Terminate the macro with an M99 code.
Use local variables within the body of a macro or subprogram only. You
cannot use them to transfer data to other macros or subprograms. If
further subprogram calls are made from the macro body, you must
transfer data from the local variables to common variables. The common
variables can then be referenced to transport data to the further
subprogram.
All rights reserved. Subject to change without notice.
17-April-04
19-13
CNC Programming and Operations Manual
P/N 70000487G - Advanced Programming Features
N220 #100 = #20
N230 ------Common variables range from #100 to #220.
The macro must either be part of the program from which it is called or
"included" using the file inclusion code. Refer to “File Inclusion” in this
section.
Setting and Passing Parameters
You can set parameters for a macro before the subprogram call (M98
Pn). Refer to Example 1. Blocks 10 to 12 define variable values for the
subprogram called in Block 13.
Example 1
N10
N11
N12
N13
N14
#151 = 2
#152 = 3
#153 = 3.4
M98 P1
-------
It may be more convenient to use macro call G65 Pn or G66 Pn to pass
variables to the subprogram by letter address. This is how a canned cycle
operates. Refer to Example 2. Values are passed on for parameters A,
B and C.
Example 2
N20
N21
G65 P1 A2 B3 C3.4
-------
Macro call G65 Pn contains a loop option (Ln). Where, n is the number
of repetitions of the subprogram called.
N20 G65 P1 A2 B3 C3.4 L3
N21 ------Macro 1 will be called three times (Ln equals 3).
When parameters are passed to a macro body by letter address, the
contents of the parameters are stored in local variables. Refer to
Table 19-5.
Table 19-5, Letter Addresses
A = #1
H = #11
R = #18
X = #24
B = #2
I = #4
S = #19
Y = #25
C = #3
J = #5
T = #20
Z = #26
D = #7
K = #6
U = #21
E= #8
M = #13
V = #22
F = #9,
Q = #17,
W = #23,
Letter addresses G, L, N, O, and P cannot be used for parameter
passing.
19-14
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Advanced Programming Features
G65 Macro Programming, Main
The following is an example of a simple macro program. In this example,
the macro is a "window milling" cycle designed to mill a square or
rectangular window through a part.
Example:
N1
N2
N3
N4
N5
N6
N7
N8
N9
N10
N11
N12
N13
N14
N15
O99 * WINDOW-MACRO-CALL
G90 G70 G0 G17
T0
Z0
X0 Y0
T1 *** .5000 MILL
G90 G0 X1 Y1
Z.1
F40
G65 P3 X4 Y4 Z-.55
G90 G0 Z.1
T0
Z0
X0 Y0
M30 O99
* parameters passed:
* X (#24) = length of window in X axis
* Y (#25) = width of window in Y axis
* Z (#26) = absolute tool depth
All rights reserved. Subject to change without notice.
17-April-04
19-15
CNC Programming and Operations Manual
P/N 70000487G - Advanced Programming Features
G65 Macro Programming, Macro (Subprogram)
This macro can mill any size window (L x W), at any Z depth. To change
the pocket size, change the parameters on Block 10 (X,Y,Z). The CNC
will execute the macro only once, at the current position. (G65 is not
modal.)
Example:
N22
N23
N24
N25
N26
N27
N28
N29
N30
N31
O3 * WINDOW-MACRO
G90 G1 Z#26
G91 G41 Y(#25/2)
X(-(#24/2))
Y(-#25)
X#24
Y#25
X(-(#24/2))
G40 Y(-(#25/2))
M99
G66/G67 Macro Programming
This example is a modal macro program to mill slots in a plate at various
locations. In contrast to the G65 (single-call macro) in Example 1, G66
(modal macro call) applies the macro to all subsequent moves, until
canceled by G67. Program G67 after the last slot location.
Example:
N1
N2
N3
N4
N5
N6
N7
N8
N9
N10
N11
N12
N13
N14
O101 * SLOTCALL.G
G90 G70 G0 G17
T0 Z0
X0 Y0
T1 D.25 L-1 F30
G66 P1255 X5 Y1 Z-.1 A5 B12 C5
X1 Y2
X2 Y4
G67
G90 G0 T0 Z0
X0 Y0
M2
["SLOTMAC.G
This program calls SLOTMAC.G, a program in another file. The "file
inclusion" block (N14) calls the program from another file in the Program
Directory.
19-16
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Advanced Programming Features
SLOTMAC.G Program
In the following Blocks 1260 through 1400 are comment blocks that
regard the macro's structure and concept.
Example:
N1255
N1260
N1270
N1280
N1290
N1300
N1310
N1320
N1330
N1340
N1350
N1360
N1370
N1380
N1390
N1400
N1410
N1420
N1430
N1440
N1450
N1460
N1470
N1480
N1490
N1500
N1510
N1520
N1530
O1255 * SLOTMAC.G
* EXAMPLE: G65 P1255 X-3 Y1 Z-.125 A5 B12 C10
* P = SUB #
* X = X DIM OF SLOT
#24
* Y = Y DIM OF SLOT
#25
* Z = ABS DEPTH OF SLOT #26
* A = Z FEEDRATE
#1
* B = XY FEEDRATE
#2
* C = ANGLE FROM 3 o’clock #3
* NOTES:
* 1. SLOT WILL HAVE FULL RAD.
* 2. MUST POS'N XY OVER CENTER OF L.LEFT RAD.
* 3. PROGRAM SLOT LENGTHWISE IN X, ANGLE C WILL ROTATE
G90 G0 Z.1
G61 Z#26 F#1
G68 C#3
G91 G41 G64 X.1 Y(#25/2) F#2
X-.1
G3 X0 Y(-(#25)) I0 J(-(#25/2))
G1 X(ABS((ABS(#24))-(ABS(#25))))
G3 X0 Y#25 I0 J(#25/2)
G1 X(-(ABS((ABS(#24))-(ABS(#25)))))
G1 G40 Y(-(#25/2))
G68
G90 G0 Z.1
M99
All rights reserved. Subject to change without notice.
17-April-04
19-17
CNC Programming and Operations Manual
P/N 70000487G - Advanced Programming Features
Macro Programming (Hole Milling Macro)
Example 3 machines a CW or CCW hole. A move is made to the hole
center and to the required Z depth before calling the macro. After the
macro is completed, the Z-axis moves to the clearance plane. The macro
contains tangential entry to and exit from the hole surface. It uses error
checking and messages. When the macro is finished, machine
parameters return to the their previous status.
String variables (Examples: EPSI, SAVEFRT) can be set and used in
place of regular variables.
String Variables
String variables can be used to make a macro program easier to
understand. They can represent a value or a variable. They can be used
only in subprograms.
String variables must be set before use, in the following format:
[ TEXT value or variable
Examples:
[ PI 3.141592654
*PI will be read as the value given
[ TFLAG #1041
*TFLAG will represent system variable
#1040 (current tool comp)
NOTE: Open bracket must start line. Do not use equal signs (=) in
string variables.
You can use a variable to print values.
#35= PI ;print 35
*3.141592654 will be printed
There must be at least one space preceding and following the string
variable in a program. In the following examples, PI is the variable.
#35/PI+#23
Produces error.
#35/ PI +#23 Correct format.
Once set, string variables can be used in any macro within the same
program.
Example:
G90 G70 G0 G17
T0 Z0
X0 Y0
T1 F30
X1.5 Y0 * MOVE TO HOLE CENTER
Z.1
G1 Z-.5 * MOVE Z TO DEPTH
G65 P76 D2.0 S.010 J35 K20
G0 Z.1 * RAISE Z TO CLEARANCE PLANE
19-18
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Advanced Programming Features
TO Z0
X0 Y0
M2
O76 ** HOLE MILLING MACRO.
*
* D#7 = HOLE DIAMETER (+=CCW,-=CW), J#5 = ROUGH FEEDRATE,
* S#19 = FINISH STOCK AMOUNT, K#6 = FINISH FEEDRATE.
* #1020 = TOOL DIAMETER.
*
[SAVEG90 #99 * SET STRING SAVEG90 TO VAR 99
[SAVEG00 #98 * SET STRING SAVEG00 TO VAR 98
[SAVEFRT #97 * SET STRING SAVEFRT TO VAR 97
[TDIA #96 * SET STRING TDIA TO VAR 96
[EPSI .00001 * SET STRING EPSI TO .00001
SAVEG90 = #1090 * SAVE CURRENT DIM MODE (ABS=90,INCR=91)
SAVEG00 = #1016 * SAVE CURRENT MOVE MODE (RAPID=0,FEED=1)
SAVEFRT = #1022 * SAVE CURRENT FEEDRATE
TDIA = ABS(#1020) * SAVE CURRENT ABSOLUTE TOOL DIA
IF(!VAR(7)) THEN
PRINT (ERROR! HOLE DIA. NOT GIVEN)
M30
ENDIF
IF(!VAR(5)) THEN; #5=#1022; ENDIF * DEFAULT ROUGH FEEDRATE.
IF(!VAR(6)) THEN; #6=#5; ENDIF * DEFAULT FINISH FEEDRATE.
IF(!VAR(19)) THEN; #19=0.; ENDIF * DEFAULT NO FINISH STOCK.
IF(ABS(#7/2)<ABS(#19)) THEN
PRINT (ERROR! TOOL DIA. TOO BIG)
M30
ENDIF
#33 = (ABS(#7)/2-ABS(#19)- TDIA /2); * ROUGHING PASS RADIUS.
IF(#33<0|#33=0) THEN
PRINT (ERROR! ROUGH AMOUNT TOO BIG)
M30
ENDIF
IF( #1041 > 40+ EPSI ) THEN * CHECK IF TOOL COMP IS ON
PRINT (ERROR! TOOL COMP NOT ALLOWED)
M30
ENDIF
IF( TDIA < EPSI ) THEN
PRINT (WARNING: TOOL DIA.= 0)
M00 * DWELL UNTIL START KEY.
ENDIF
#34 = (#33/2); * INTERMEDIATE RADIUS.
#35 = (ABS(#7)/2- TDIA /2); * FINISH PASS RADIUS.
#36 = (#35/2); * INTERMEDIATE RADIUS.
G64; * CONTOURING MODE.
IF(#7>0) THEN * COUNTER-CLOCKWISE.
G91 F#5
G01 X#34 Y#34
All rights reserved. Subject to change without notice.
17-April-04
19-19
CNC Programming and Operations Manual
P/N 70000487G - Advanced Programming Features
G03 X(-#34) Y#34 I(-#34) J0
G03 X0 Y0 I0 J(-#33)
G03 X(-#34) Y(-#34) I0 J(-#34)
G01 X#34 Y(-#34)
IF((#19> EPSI ) & (#6> EPSI )) THEN * IF FINISH PASS.
G91 F#6
G01 X#36 Y#36
G03 X(-#36) Y#36 I(-#36) J0
G03 X0 Y0 I0 J(-#35)
G03 X(-#36) Y(-#36) I0 J(-#36)
G01 X#36 Y(-#36)
ENDIF
ELSE * CLOCKWISE.
G91 F#5
G01 X(-#34) Y#34
G02 X#34 Y#34 I#34 J0
G02 X0 Y0 I0 J(-#33)
G02 X#34 Y(-#34) I0 J(-#34)
G01 X(-#34) Y(-#34)
IF((#19> EPSI ) & (#6> EPSI )) THEN * IF FINISH PASS.
G91 F#6
G01 X(-#36) Y#36
G02 X#36 Y#36 I#36 J0
G02 X0 Y0 I0 J(-#35)
G02 X#36 Y(-#36) I0 J(-#36)
G01 X(-#36) Y(-#36)
ENDIF * FINISH PASS.
ENDIF * CLOCKWISE
IF( SAVEFRT > EPSI ) THEN; F( SAVEFRT ); ENDIF * RESTORE FEEDRATE.
G SAVEG90 ; * RESTORE G90/91.
G SAVEG00 ; * RESTORE G00/01.
M99
19-20
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Advanced Programming Features
Probe Move (G31)
G31 is to be issued with an associated axis move (i.e. G31 X10). When
the G31 is executed, it moves at current feedrate selected for G1 until the
touch probe selected is deflected. At this point, the move is stopped, and
the position where the probe touched the part is read and passed to
system variables (#1060 to #1063 for X to U).
G31 is aborted if any of the following events occur:
• The primitive is issued while the probe is still deflected (touching the
part).
• The ready signal is not present.
• Hardware malfunction: Trigger signal engaged, but no position is
latched.
• Start pulse is issued, but probe is not ready after 2 seconds. (Only
cordless probes).
• Cordless probe still in “sleeping mode.”
• Low battery signal becomes active (Only cordless probes).
M-code M9387 is provided to select the probe G31 will use and probe
activation:
M9387X0
M9387X1
M9387Y0
M9387Y1
M9387Z0
M9387Z1
Selects the Tool touch probe (X13)
Selects the 3-D touch probe (X12) (default)
Copies Tool touch probe state (deflected or not) into a
system variable (#1066)
Copies 3-D touch probe state (deflected or not) into a
system variable (#1066)
Turns off cordless probe
Turns on cordless probe
Canned cycles are available for the most common probe functions. Refer
to Probing Cycles, P/N 70000557, for details. Using the G31 primitive,
parametric programming and the M-code described above, it is possible
to write additional cycles to perform custom probing functions.
All rights reserved. Subject to change without notice.
17-April-04
19-21
CNC Programming and Operations Manual
P/N 70000487G - Advanced Programming Features
Conditional Statements
This subsection discusses the conditional statements IF, THEN, ELSE,
GOTO and WHILE.
IF - THEN - ENDIF
N300 IF (expression) THEN
N310 ------------------::
::
N360 ENDIF
N370 --------If the expression in N300 is true, the program continues at N310. If the
expression is false, the program continues at N370.
In place of an expression, you can use a variable that while not zero will
be treated as a true expression. (Zero equals false. Any other value
equals true.)
IF - THEN - ELSE - ENDIF
N400 IF (expression) THEN
N410 ------------------::
::
N440 ELSE
N450 ------------------::
::
N470 ENDIF
N480 --------If the expression is true, the program continues at N410, then to N440,
where a jump is made to N480.
If the expression is false, the CNC skips Blocks N410 to N440 and
executes Blocks N450 to N470. In place of an expression, you can use a
variable that while not zero will be treated as a true expression. (Zero
equals false. Any other value equals true.)
IF - GOTO
N500 IF (expression) GOTO nnnn
N510 --------NOTE: When you program IF-GOTO statements do not precede the
block number with the character "N".
For example, IF-GOTO 487 skips to block number N487.
If the expression is true, the program jumps to the block number specified
(nnn). If the expression is false, the program continues at Block N510.
In place of an expression a variable can be used which while not zero will
be treated as a true expression. (Zero equals false. Any other value
equals true.)
19-22
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Advanced Programming Features
WHILE - DO - END
N550 WHILE (expression) DO nnnn
N560 -----------------------::
::
N590 END nnnn
N600 --------If the expression is true, the program repeats between N550 and N590
until the expression becomes false. Similarly, if the expression is false
when Block N550 is executed, the CNC jumps to Block N600. The
number after DO is a label (identifier only) and the same number must be
used to identify the END of the loop.
In place of an expression, you can use a variable that while not zero will
be treated as a true expression. (Zero equals false. Any other value
equals true.)
DO - END
N620 DO nnnn
N630 --------::
::
N650 IF ( expression ) GOTO 1111
N660 ------------------N670 END nnnn
DO - END sets the program into an infinite loop that can only be ended
by programming a GOTO (1111) command to another block. DO and
END must be paired with labels (nnnn). When executed the program will
repeat Blocks N630 to N660 until the expression at N650 becomes true
and program execution continues at block (1111).
Unconditional LOOP Repeat
Conditional statements require that a test be strictly true or false in order
for a particular course of action to be taken. Unconditional statements
are acted on without a logical precondition.
LOOP - END
N680 LOOP nnnn
N685 --------::
::
N695 END
LOOP instructs the control to execute the following blocks (N685) until it
reaches an END command. The sequence is repeated nnnn times. The
number of loops can be a variable assignment ( LOOP #121 ).
All rights reserved. Subject to change without notice.
17-April-04
19-23
CNC Programming and Operations Manual
P/N 70000487G - Advanced Programming Features
GOTO
\N698 GOTO nnnn
N699 ---------GOTO is an instruction to continue program execution at the block
specified (nnnn). You should not require this instruction in a user macro.
It is intended for use in conjunction with the block skip symbol (\), as
shown in the example. When block skip is ON, Block N698 is not
executed. When block skip is OFF, Block N698 is executed and program
execution jumps to the block specified.
NOTE: When you program GOTO statements do not precede the block
number with the character "N".
For example, GOTO 610 skips to block number N610.
Short Form Addressing
The appropriate abbreviation instructs the CNC to activate the
corresponding command. Refer to Table 19-6.
Table 19-6, Abbreviations
Command
DO
END
GOTO
IF
LOOP
PRINT
THEN
WHILE
19-24
Abbreviation
]D
]E
]G
]I
]L
]P
]T
]W
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Advanced Programming Features
Logical and Comparative Terms
Logical Terms
All logical operations can be carried out using the following command
characters or combinations of characters. Refer to Table 19-7.
Table 19-7, Logical Symbols
Statement
Symbol
OR
EXCLUSIVE
OR
^
AND
&
True/False Table
0-0 = False
0-1 = True
1-0 = True
1-1 = True
0-0= False
0-1= True
1-0= True
1-1 = False
0-0= False
0-1= False
1-0= False
True
Comparative Terms
You can compare variables with variables and variables with constants
using equality and inequality operators.
Equality Operators
N700 IF (#120 = #125) THEN (or GOTO)
N710 -------------------::
::
N740 IF (#130 = 360) THEN (or GOTO)
N750 -------------------Block N700 compares the contents of variable #120 with the contents of
variable #125. If the contents are equal, then the expression is true and
THEN or GOTO directs the program. Otherwise, the expression is false.
At Block N740, the contents of variable #130 are compared with the
constant 360. The result of the comparison is identical to the first case.
All rights reserved. Subject to change without notice.
17-April-04
19-25
CNC Programming and Operations Manual
P/N 70000487G - Advanced Programming Features
Inequality Operators
NOT
N760 WHILE (#135 != #137) DO 10
N770 -----------------------::
N790 END 10
The exclamation mark (!) symbolizes NOT. Therefore, Block N760
instructs the CNC to continue the loop to N790 while the contents of
variables #135 and #137 are not equal (condition true). When the
contents of the variables become equal the expression is false and the
loop terminates.
GREATER THAN
N800 IF (#122 > #134) GOTO 830
N810 -------------------The symbol (>) symbolizes GREATER THAN. Therefore, Block N800
instructs the control to go to (GOTO) or jump to Block N830 if the
contents of variable #122 are greater than the contents of variable #134
(condition true). If the expression is false, execution continues to Block
N810.
LESS THAN
N840 IF (#123 < #135) GOTO 880
N850 -------------------The symbol (<) symbolizes LESS THAN. The function is the opposite of
GREATER THAN and the expression is true when the contents of
variable #123 are less than the contents of variable #135.
NOTE: Greater than (>) and less than (<) expressions become false if
the contents of the compared variables are equal.
File Inclusion
Example 1: ["FILENAME.G
File inclusion is a function that allows a subprogram that is not actually
part of the file to be called from the main program, or from another
subprogram in the file.
In this way, a tool change subprogram or a macro can be stored in the .G
directory, and called from any other program that has the proper "file
inclusion" code, which will allow the execution of the external
subprogram.
Example 1 shows the syntax necessary to "include" a file into another file.
Format: open left bracket ([), then double quote character ("), then the
filename and its extension. This line must appear somewhere in the
program that is to call the "included" program.
19-26
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Advanced Programming Features
Example 2:
N1 O23 * TEST.G
N2 M98 P9
N3 T1 * 1.0000 MILL
N4
G0 X-.6 Y.6
N5 Z.1
N6 .
N7 .
.
.
.
N33 M98 P9
N34 T2
N35 * .368 DRILL
N36
.
.
.
N50 M98 P9
N51 M30 O23
N52 ["TOOLCHNG.G
In Example 2, a program named TOOLCHNG.G can be called from the
main program (or from an existing subprogram). It is made possible by
line N52. The file inclusion function is programmed on N52.
In this way, the same subprogram can be used in many programs, but
you do not need to type it into each program. Each program must,
contain the proper "file inclusion" block.
The program to be included must be in the form of a subprogram,
beginning with Onnn, and ending with the M99 code.
The format for file inclusion is: ["FILENAME.G
It is especially useful for including tool change subprograms, zero-setting
subprograms and macros.
All rights reserved. Subject to change without notice.
17-April-04
19-27
CNC Programming and Operations Manual
P/N 70000487G - Index
% Executing Buffer Full, 13-10
% Feed, machine status display,
3-6
% Receiving Buffer Full, 13-10
% RPM, machine status display,
3-6
*, wildcard, 10-11
.fxd extension, created, using
DXF converter, 17-11
.G extension, 10-3, 10-5
created, using DXF converter, 17-1,
17-11
.M extension, created, using
DXF converter, 17-1, 17-11
.S files, 10-4
?, 10-11
6000M CNC Setup Utility
Manual, P/N 70000490,
referenced, 3-14
A
abbreviating statements, 6-10
abbreviations, command, listed,
19-24
absolute mode
center-angle arc, illustration, 7-16
change to, (G90), 4-29
description, 1-5, 3-9
absolute zero
defined, 3-9
point, to set, (G92), 4-30
reference point, 1-5, 3-9
accessing, communication
software, 13-2
accessing, DNC, 13-10
activate
4th (U) axis synchronization, (M900), 12-4
manual mode, feed, 3-8
manual mode, rapid, 3-8
plane rotation at pre-set value, (M801),
12-4
servos, 3-2
test link screen, 13-6
active soft key, manual screen
area, 3-6
address words, typing in, 7-34
adjusting
Draw display, 8-9
All rights reserved. Subject to change without notice
17-April-04
feedrate, 4-31
rapid move speed, 3-8
advance block
beginning, 6-6
end of, 6-6
end of program, 6-6
first of program, 6-6
advanced programming features
block, separators, 19-1
conditional statements, 19-22
expressions, functions, 19-4
logical and comparative terms, 19-25
modifiers, description, 19-1
modifiers, listed, 19-1
probe move (G31), 19-21
system variables, 19-6
tool offset, modification, 19-2
user macros (G65, G66, G67), 19-13
user variables, 19-7
advanced scaling, (M701), 12-3
alphanumeric keys
description, 2-2
illustration, 2-2
listed, 2-3
angle of cut, parameter, 18-18
angle, measurement, 1-6
angle, references, 1-7
angular motion programming,
example, 4-5
approach height, parameter,
18-11
arc
direction, illustration, 1-8, 4-12
feedrate override, automatic, (G62, G63),
4-21
programming, description, 7-15
reverse, direction, 18-6, 18-38
segment tools, illustration, 18-36
template, illustration, 18-36
tools, table, 18-36
ARCS Help Template Menu,
parameters, table, 7-17
area clearance, irregular pocket
milling, (G169), 5-27
ARROW , keys, 2-5
arrows, parameter, 18-26
ASCII, data type, 13-5
ATC. See automatic tool
changer
Index-1
CNC Programming and Operations Manual
P/N 70000487G - Index
Auto (F6), 3-7
auto mode
program, cancel, 11-5
program, hold, 11-5
program, to run, 11-4
screen, illustration, 11-4
starting block, select
using arrow keys, 11-5
using SEARCH, 11-5
switch from, single-step mode, 11-3
AUTOEXEC.BAT, DXF
converter, example, 17-1
AUTOJOG (F1), 11-14
automatic
Draw restart, 8-7
feedrate override, arcs, (G62, G63), 4-21
mode, defined, 11-1
mode, Draw, 8-6
tool changer, 5-11, 9-4
tool changes
new tool, 18-31
to output, 18-30
auxiliary
axis, synchronous or non-synchronous,
16-2
keyboard, entity information, to display,
17-7
axes
approach, 5-34
of rotation, illustration, 5-49
parameter, description, 18-26
axis
address, unary minus, example, 19-9
descriptions, 1-3
of motion, illustration, 1-3
rotation
(G68), 4-25
(G68), canceled by G92, 4-30
G68, examples, 4-26
scaling, (G72), 4-29
scaling, (G72), canceled by G92, 4-30
select key, illustration, 3-3
selecting, 3-10
synchronization, 12-4
types
description, 16-1
linear, description, 16-1
rotary, description, 16-1
Index-2
B
ball end mill
length offsets, using, 9-12
tool diameter compensation, using, 9-12
baud rate, setting, 13-3
BINARY, data type, 13-5
Blk, program area label, 3-6
block
copy, to program, 6-16
end of program, feature, 6-6
end of, feature, 6-6
go to, feature, 6-7
number, 3-6
selected, run Draw, 8-8
separators, description, 19-1
skip variables, description, 19-7
start of program, feature, 6-6
start of, feature, 6-6
bolt hole circle, (G79), 5-13
boring. See also, drilling
bi-directional, (G85), 5-9
canned cycles, (G81–G89), 5-5
counter cycle, (G82), 5-6
example, 5-11
flat bottom bi-directional, (G89), 5-11
unidirectional, (G86), 5-9
Both, Draw, description, 8-5
bottom of contour, parameter,
18-11
buffers, CNC, 13-10
C
calc distance, soft key, 18-41
calibrate, soft keys, change
fixture offset, 4-18
CalibX, description, 4-18
CalibY, description, 4-18
CalibZ, description, 4-18
CAM
pockets with islands
Draw mode, illustration, 18-83
pocket parameters pop-up menu,
illustration, 18-83
pockets with islands, (G162), 18-21,
18-82
CAM mode
changing, view, 18-40
description, 18-1
hot keys, listed, 18-31
screen displays, table, 18-1
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Index
screen illustration, 18-2
Shape Edit Menu (F3), listed, 18-4
soft keys, listed, 18-3
soft keys, Shape (F2), listed, 18-3
soft keys, to activate, 18-2
CAM point, parameter, 18-19
CAM post processor, automatic
tool changes, to output, 18-30
CAM programs, samples, 18-48
CAM shapes
to create, 17-21
to view, 17-21
cancel
a single step run, 11-2
auto mode program, 11-5
Draw, program, 8-3
drill, tap, bore cycle, (G80), 5-6
In-Position Mode, modal, exact stop
check, (G64), 4-11
canned cycles
defined, 5-4
drilling tapping, boring, (G81–G89), 5-5
tapping, G84, 5-8
cavity detail, illustration, 5-59
chaining geometry elements, to
create shape, 18-46
chamfer tool, to use, 18-37
chamfer, a corner, 18-37
chamfering, (G59, G60), 4-19
change word, feature, 6-8
changing
CAM mode view, 18-40
jog mode, 3-10
link test link screen data display, 13-6
character, deleting, 6-4
chip-breaker peck-drilling cycle,
(G87), 5-10
circle tools, templates, listed,
18-45
circular interpolation
absolute mode, 4-7
circle, example, 4-9
incremental mode, 4-7
parameters, 4-6
partial arc, example, 4-7, 4-8
circular pocket milling, (G77),
5-23
circular profile cycle, (G171),
5-36
clear, (M9351), 12-4
All rights reserved. Subject to change without notice
17-April-04
clear, (X302), 12-4
CLEAR, key, 2-5
clearing
a halted program, 11-5
entries, 2-7
messages, 2-8
receive area, 13-7
transmit area, 13-7
clockwise motion (G2),
description, 4-6
CNC
DXF converter
description, 17-3
file creation, 17-1
files created, 17-11
enlarged motion display, to set, 11-7
parts counter, description, 11-11
software, tracks tools, 9-5
timer, description, 11-11
codes, order of execution, 12-4
colinear lines
defined, 18-6, 18-38
join, 18-7, 18-39
COM1, 13-3
COM2, 13-3
Comm Port, selecting, 13-3
command line, manual screen
area, 3-5
command, abbreviations, listed,
19-24
COMMAND, program area label,
3-6
commands, multiple move
command, 7-21
Comment, parameter, 18-12,
18-13, 18-14, 18-15, 18-18,
18-19, 18-20, 18-23, 18-24
comments, include in program
listing, 6-17
common (global) variables,
description, 19-7
communication
description, 13-1
parameters, setting, 13-3
port, to select, 13-3
screen layout, description, 13-2
screen, accessing, 13-2
screen, illustration, 13-2
software, accessing, 13-2
Index-3
CNC Programming and Operations Manual
P/N 70000487G - Index
comparative terms, description,
19-25
compensated move, ramping,
9-11
compensation
help graphic templates, listed, 7-11
left-hand, 9-9
right-hand, 9-9
COMPENSATION Help Graphic
Template Screen, parameters,
table, 7-11
completed program, 3-6
computation, storing result,
19-10
conditional statements,
description, 19-22
conical elbow details, illustration,
5-60
console, illustration, 2-1
construction geometry, using,
18-42
continuous
downloading (DNC), 13-9
jog, 3-7
jog, Feed mode, 3-10
jog, Rapid mode, 3-10
path, override, 12-4
continuous path mode. See also,
contouring mode
contour
bottom of, parameter, 18-11
description, 18-8
Parameters 1 Menu, parameter,
description, 18-10
Parameters 2 Menu, parameter,
description, 18-12
Parameters Menu, illustration, 18-9
screen, soft keys, listed, 18-15
top of, parameter, 18-11
with many unknown intersections
all tangent arcs, machining, 18-61
machining, 18-59
contouring mode, G64, 4-22
control M-codes
description, 12-2
listed, table, 12-2
conventional
jog, 3-7
jog mode, 3-10
jogging, 3-11
Index-4
conversion formula
minutes to decimal, 16-1
seconds to degrees, 16-1
COOL ON (F7), 11-15
coolant
at start, parameter, 18-14
off, (M9), 12-2
on, (M8), 12-2
ready, 3-4
COOLOFF (F8), 11-15
copy
entire program, 6-16
program blocks, 6-11
programs to floppy disks, 10-8
programs, other directories, 10-12
shape, 18-5
core detail, illustration, 5-59
corner radius tool, to use, 18-37
corner rounding/chamfering,
(G59, G60), 4-19
counter bore cycle, G82, 5-6
counterclockwise motion (G3),
description, 4-6
create
new programs, 10-2
shape, 18-4
subdirectory, 10-13
Create (F2), 10-2
current, operating mode, 3-6
cursor
edit screen, location, 6-2
tool page, description, 2-7
cutting cavity, more than one
pass, illustration, 5-50
cutting direction, 5-34
cutting mode. See also,
contouring mode
D
data bits, to set, 13-4
data control codes
function, table, 13-8
receive mode, to use, 13-9
send mode, to use, 13-9
to use, 13-8
data link, testing, 13-5
data type, to set, 13-5
date and time, 10-2
DE-9, 13-1
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Index
deactivate
4th (U) axis synchronization, (M901), 12-4
advanced scaling, (M700), 12-3
plane rotation and set angle, (M800), 12-4
decimal points, 7-10
defining, positions, 1-4
Del (F4), 2-7
DelAll (F9), 18-47
delete
a character, 6-4
a program, 10-5
all geometry elements, 18-47
geometry elements, 18-47
groups of programs, 10-7
program block, 6-4
program on another drive, 10-14
segment, forward end of shape, 18-39
shape, 18-38
text, 2-7
Delete (F3), 10-5
Delete (F7), 3-7
Delete, CAM mode, description,
18-24
DelGeom (F9), 18-47
DelMove (F8), description, 18-8
DIA, machine status display, 3-6
diameter offset, tool page, 9-8
dimensions, parameter, 18-25
direct numeric control. See DNC
direct transfer, variables, 19-9
direction of cut, parameter,
18-19
disable dry-run, (M107), 12-3
disable feed hold, (M20), 12-2
disabled, features, off-line, 15-3
disclaimer, iii
disengage, servos, 3-1
disk optimizer, to access, 10-15
display
Draw, adjusting, 8-9
Draw, fit window, 8-9
Draw, scale, 8-9
erase, 8-7, 8-12
modes, listed, 10-2
size
double, 8-11
half, 8-11
to change, 8-11
zoom in, 8-10
DISPLAY (F5), 8-1
All rights reserved. Subject to change without notice
17-April-04
DNC
mode, for CNC, 13-11
running, 13-9
screen, illustration, 13-10
to access, 13-10
Double, display function, 18-40
draft angle pocket cycle, (G73),
5-17
Draw
automatic mode, 8-6
CAM, pockets with islands, illustration,
18-83
CNC code, view tool paths, 17-3
display
adjusting, 8-9
erase, 8-12
fit window, 8-9
size
double, 8-11
half, 8-11
scale, 8-9
end at, specific block, 8-8
erase display, 8-7
grid parameter, to set, 8-6
grid size, to set, 8-6
motion mode, 8-6
parameters, viewing, 8-4
rapid moves, description, 8-5
real-time mode, description, 8-1
restart, automatic, 8-7
run, selected block:, 8-8
S.Step, 8-6
simulation mode
cancel, program, 8-3
description, 8-1
operation mode, 8-2
screen, illustration, 8-2
status items, listed, 8-3
to activate, 8-2
to pause, 8-3
single-step mode, 8-6
start at, specific block, 8-8
starting, 8-1
tool compensation, description, 8-5
tool, on or off, 8-4
ToolComp, description, 8-5
using while running programs, 11-6
view area, change, 8-11
viewing, programs, 8-1
window, zoom, 8-10
Index-5
CNC Programming and Operations Manual
P/N 70000487G - Index
Draw (F7), 8-1
Drawing Exchange File. See
DXF converter
drill
(sync-off), programming examples, 16-4
cycle, parameter, 18-23, 18-26
function, description, 18-21
Drill Parameter Menus,
illustration, 18-22
Drill Parameters 1 Menu,
parameters, listed, 18-23
DRILL/TAP Help Template
Menu, parameters, table, 7-29
drilling. See also, boring
drilling, tapping, boring canned
cycles, (G81–G89), 5-5
drives, log on, 10-6
dry-run
all axes, (M105), 12-3
disable, (M107), 12-3
NO Z-axis, (M106), 12-3
OFF (M107), 12-3
dwell, 5-8
dwell (G4), description, 4-10
DWELL, machine status display,
3-6
DXF converter
CNC code, description, 17-3
contours and drill holes, 17-1
contours, description, 17-3
convert polyline, description, 17-9
create, conversational file, 17-1
create, G-code file, 17-1
display menu, descriptions, 17-9
drilling, description, 17-3
edited
conversational program, listing, 17-15
g-code program, listing, 17-17
g-code tool path, illustration, 17-16
entities supported, table, 17-10
entities, not supported, 17-10
entity endpoints, toggle, 17-5
example, 17-11
exit (F10), description, 17-7
feature, description, 17-1
files, created, 17-11
hot keys, table, 17-5
mouse operations, table, 17-4
output format, pop-up menu, 17-18
output menu, descriptions, 17-8
Index-6
output menu, example, 17-12
pockets with islands (G162)
description, 17-18
program example, 17-20
program listing, pop-menu, 17-19
requirements
machine software, 17-1
off-line software, 17-1
shapes
creating, 17-2
types, listed, 17-2
shift X, shift Y, descriptions, 17-8
soft keys, descriptions, 17-6
to open, 17-2
troubleshooting, 17-5
unedited, conversational program listing,
17-13
unedited, g-code program listing, 17-14
E
edit
canceling unsaved, 6-4
function, description, 18-24
help
description, 7-1
M-code listing, 7-33
screens, illustration, 7-2
soft keys, listed, 7-7
keys, illustration, 2-2
keys, table, 2-5
program in another directory, 10-15
program, feature, 6-15
saving, 6-4
screen, description, 6-2
shape, soft keys, 18-37
soft keys, description, 6-2
tools, selecting, 18-32
Edit (F3), 3-7
Edit Help G-Code Menu, table,
7-32
edited marker, description, 6-2
effectivity notation, 1-1
elbow cavity & core, illustration,
5-57
elbow milling cycle
execution, illustration, 5-57
G49, description, 5-56
illustration, 5-58
ellipse programming, illustration,
5-1
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Index
ellipse, G5, 5-1
ELSE, conditional statement,
19-22
emergency stop, reset, 3-1
enable feed hold, (M21), 12-2
End N#, parameter, 8-8
end of
block, feature, 6-6
program, feature, 6-6
subprogram, (M99), 5-65
end user, common (global)
variables, macro numbers,
19-7
enlarged motion display, set the
CNC, 11-7
ENTER, key, 2-5
entity information
DXF miscellaneous menu (F6),
description, 17-7
off-line, to display, 17-7
to display, DXF miscellaneous menu (F6),
17-7
entries, clearing, 2-7
entry / exit moves, parameter,
18-13
entry field types, listed, 7-10
equality operators, description,
19-25
erase, display, 8-12
Erase, display function, 18-40
Erase, parameter, 8-7
error messages, displayed, 2-8
E-STOP
emergency stop, 3-1
key, illustration, 3-4
no keyboard equivalent, 14-1
to reset, 3-1
exact stop check
G61, In-Position Mode, modal, 4-21
G64, cancel (G61), 4-21
G9, In-Position Mode, non-modal, 4-21
G-Code, formats, 4-11
non-modal, G9, 4-11
examples
jog/return, 11-16
practice, 18-85
exit
(F10), description, 18-31
(F10), DXF converter, 17-7
off-line software, 15-1
All rights reserved. Subject to change without notice
17-April-04
shut down, 3-1
EXIT (F10), 3-8
Exit (Shift + F10), 3-8
expand key, feature, 6-10
expressions
description, 19-4
examples, 19-5
listed, operators, 19-4
unary minus, example, 19-9
F
F1 (AUTOJOG), 11-14
F1 (Help), 3-7
F1 (Message), 3-8
F1, toggle select mode, DXF
converter, 17-6
F10 (Exit), 3-8
F10 (Handwheel, 3-8
F10, exit, DXF converter, 17-7
F2 (Create), 10-2
F2 (Program), 3-7
F3 (Delete), 10-5
F3 (Edit), 3-7
F3 (Ins), 2-7
F3 (ZHOME), 11-14
F3, layers menu, DXF converter,
17-6
F4 (Del), 2-7
F4 (Manual), 3-7
F4 (MANUAL), 11-14
F4, view menu, DXF converter,
17-6
F5 (Display), 8-1
F5 (S.Step), 3-7
F5 (Teach), 3-8
F5, display menu, DXF
converter, 17-6
F6 (Auto), 3-7
F6 (RETURN), 11-15
F6, miscellaneous menu, DXF
converter, 17-6, 17-7
F7 (COOL ON), 11-15
F7 (Delete), 3-7
F7 (Draw), 8-1
F7 (Home), 3-8
F8 (COOLOFF), 11-15
F8 (Insert), 3-8
F8, save, DXF converter, 17-6
F9 (Parms), 8-1
F9 (Tool), 3-8
Index-7
CNC Programming and Operations Manual
P/N 70000487G - Index
F9 (TOOL), 11-15
F9, setup, DXF converter, 17-6
face cycle tool approach,
illustration, 5-34
facing cycle, (G170), 5-34
features, disabled, off-line, 15-3
feed per revolution, (G95), 4-31
FEED, machine status display,
3-6
Feed, move, 3-10
feedrate
adjustment, 4-31
in IPM, (G94), 4-30
parameter, 18-14
FEEDRATE OVERRIDE
adjusting, 3-8
setting, 3-6
switch, adjusting, 4-31
switch, illustration, 3-3
file inclusion, description, 19-26
find text, feature, 6-6
find word, feature, 6-6
first block, 1-2
Fit, display function, 18-40
fixture offset table
description, 4-17
to activate, 4-17
to adjust, 4-18
to change, 4-18
to change, using calibrate soft keys, 4-18
fixture offsets, (G53)
description, 4-17
examples, 4-18
FIXTURE, machine status
display, 3-6
flat bottom bi-directional boring,
(G89), 5-11
floppy disk
checking for lost data, 10-9
copy programs, to, 10-8
display, 10-6
rename programs, 10-12
four-axis programming,
description, 16-1
frame pocket milling, (G75), 5-19
functions
description, 19-4
listed, operators, 19-4
Index-8
G
G, machine status display, 3-6
G0, 4-1
G0, rapid traverse, description,
4-3
G1, 4-1
G1, linear interpolation,
description, 4-4
G162, pockets with islands, 5-29
G169, 4-2
G169, irregular pocket milling,
5-27
G169, programming example,
illustration, 5-32, 5-33
G17, 4-9, 4-11, 4-28, 5-45
G17, G18, G19 - plane selection,
4-11
G170, 4-2
G170, facing cycle, 5-34
G171, 4-2
G171, circular profile cycle, 5-36
G172, 4-2
G172, rectangular profile cycle,
5-38
G173, programming example,
illustration, 5-18
G177, 4-2, 5-45
G177, plunge circular pocket
milling, 5-43
G177, plunge rectangular pocket
milling, 5-44
G178, 4-2, 5-16
G179, 4-2
G179, hole pattern, 5-14
G179, programming example,
illustration, 5-15
G18, 4-11, 5-45
G181, 4-2
G181, thread mill cycle, 5-40
G19, 4-11, 5-45
G2, 4-1
G2, clockwise motion,
description, 4-6
G22, 4-1
G22, set software limits, 4-13
G28, 4-1
G28, machine home, return to,
4-15
G29, 4-1
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Index
G29, machine home, return
from, 4-16
G3, 4-1
G3, counterclockwise motion,
description, 4-6
G31, 4-1
G31, probe move, 4-16, 19-21
G4, 4-1
G4, dwell, description, 4-10
G40, 4-1, 4-19, 5-3
G40, to cancel
G41, 4-19
G42, 4-19
G40, tool compensation, cancel
mode, 9-13
G41, 4-1, 4-19, 5-2, 5-16
G41, canceled by, G40, 4-19
G41, G42, tool path
compensation, 9-9
G41, programming example,
9-21
G42, 4-1, 4-19, 5-2, 5-3, 5-16
G42, canceled by, G40, 4-19
G42, programming example,
9-22
G45, 4-1
G45, mold rotation, 5-45
G45, programming example, 554, 5-55
G49, 4-1
G49, elbow milling cycle, 5-56
G49, programming example,
5-60
G5, 4-1, 5-2
G5, ellipse, 5-1
G53, 4-1
G53, fixture offsets
description, 4-17
examples, 4-18
G59, 4-1
G59, G60, modal corner
rounding/chamfering, 4-19
G6, spiral, 5-3
G60, 4-1, 4-19
G61, 4-1, 4-22
G61, In-Position Mode, modal,
exact stop check, 4-11, 4-21
G62, 4-1
G62, G63, arc, automatic
feedrate override, 4-21
All rights reserved. Subject to change without notice
17-April-04
G63, 4-1
G64, 4-1
G64, cancel (G61), 4-21
G64, cancel, In-Position Mode,
modal, exact stop check, 4-11
G64, contouring mode, 4-22
G65, 4-1, 4-23
G65 macro program, example,
19-15
G65 macro subprogram,
example, 19-16
G65, G66, G67, user macros
description, 19-13
referenced, 4-22
G65, non-modal, 4-23
G66, 4-1, 4-23
G66, modal, 4-23
G66/G67 macro program,
example, 19-16
G67, 4-1
G68, 4-2
G68, axis rotation, 4-17, 4-25
G68, axis rotation, canceled by
G92, 4-30
G70, 4-2, 4-30
G70, inch mode format, 4-28
G71, 4-2, 4-30
G71, mm mode format, 4-28
G72, 4-2, 12-3
G72, axis scaling, 4-29
G72, axis scaling, canceled by
G92, 4-30
G72, scaling, 4-17
G73, 4-1
G73, draft angle pocket cycle,
5-17
G75, 4-1, 5-20
G75, frame pocket milling, 5-19
G75, programming example,
illustration, 5-20
G76, 4-2
G76, hole milling cycle, 5-21
G76, programming example,
illustration, 5-22
G77, 4-2
G77, circular pocket milling, 5-23
G77, programming example,
illustration, 5-24
G78, 4-2, 5-16, 5-17
Index-9
CNC Programming and Operations Manual
P/N 70000487G - Index
G78, programming example,
illustration, 5-26
G78, rectangular pocket milling,
5-25
G79, 4-2, 5-13
G79, bolt hole circle, 5-13
G80, 4-2
G80, cancel drill, tap, bore cycle,
5-6
G81, 4-2, 5-13
G81, spot drilling cycle, 5-6
G81–G89, drilling, tapping,
boring canned cycles, 5-5
G82, 4-2
G82, counter bore cycle, 5-6
G83, 4-2
G83, peck drilling cycle, 5-7
G84, 4-2, 5-5
G84, tapping canned cycle, 5-8
G85, 4-2
G85, boring, bi-directional, 5-9
G86, 4-2
G86, boring, unidirectional, 5-9
G87, 4-2
G87, chip-breaker peck-drilling
cycle, 5-10
G89, 4-2, 5-13
G89, flat bottom bi-directional
boring, 5-11
G9, 4-1, 4-22
G9, exact stop check, nonmodal, 4-11
G9, In-Position Mode, nonmodal, exact stop check, 4-11,
4-21
G90, 4-2
G90, absolute mode, change to,
4-29
G91, 4-2, 4-28, 5-3
G91, incremental mode, change
to, 4-29
G92, 4-2
G92, absolute zero point, to set,
4-30
G92, to cancel
G68, axis rotation, 4-30
G72, axis scaling, 4-30
M100, mirror image, 4-30
G94, 4-2
G94, feedrate in IPM, 4-30
Index-10
G95, 4-2
G95, feed per revolution, 4-31
G-code
defined, 4-1
directly to, Help Graphic Screen, 7-1
entering, 7-31
entering, example, 7-34
entry fields, 7-32
exact stop check, formats, 4-11
filename, parameter, 18-29
in-position mode, formats, 4-21
listed, table, 4-1
listing, table, 7-31
macros, description, 4-23
modal box, illustration, 7-30
output
repeat, 18-29
suppress, 18-29
programs, using shapes, 18-48
user macros, listed, 19-13
geometry
chaining elements, to create shape, 18-46
circle tools, templates, listed, 18-45
construction, using, 18-42
delete, all elements, 18-47
delete, elements, 18-47
elements listing, viewing, 18-46
line tools, templates, listed, 18-44
list, soft key, 18-40
notes, 18-45
options, listed, 18-27
point tools, templates, listed, 18-43
setting, description, 18-27
tools, to access, 18-42
getting started, 1-2
go to block, feature, 6-7
GOTO, conditional statement,
19-24
GREATER THAN operator,
description, 19-26
grid
parameter, 18-26
parameter, to set, 8-6
size, parameter, 18-26
size, to set, 8-6
H
Half, display function, 18-40
halted program, clearing, 11-5
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Index
HALTED/*HALTED/RUNING,
program area label, 3-6
handle mold core, illustration,
5-54
handshaking, 13-4
handwheel
jog mode setting, table, 3-14
key, illustration, 3-3
to operate, 3-13
to select, 3-13
Handwheel (F10), 3-8
hard drive, optimize, 10-15
helical interpolation
description, 4-9
example, 4-9
program, example, 4-9
Help (F1), 3-7
Help Graphic Screen
COMPENSATION, 7-11
directly to, without menus, 7-1
features, description, 7-9
illustration, 7-6
use to enter program blocks, 7-10
Help Template Menu
ARCS, 7-17
DRILL/TAP, 7-29
features, description, 7-8
illustration, 7-4
LINES, 7-14
MULTIPLE, 7-22
PATHS, 7-28
PLUNGE POCKETING, 7-27
POCKETING, 7-26
RAD/CHAMFER, 7-20
template, description, 7-5
highlight bar, 2-6
hold
a single step run, 11-2
auto mode program, 11-5
Draw, description, 8-3
the execution, 11-2
transmission / receiving operations, 13-8
Hold (F1), 13-8
HOLD key, illustration, 3-4
hole milling cycle, (G76), 5-21
hole pattern, (G179), 5-14
Home (F7), 3-8
HOME Z, description, 18-29
hot keys
CAM mode, listed, 18-31
All rights reserved. Subject to change without notice
17-April-04
DXF converter, table, 17-5
R, 18-47
R, refresh screen, 18-39
I
IF, conditional statement, 19-22
Ignore, Draw, description, 8-5
import, shape from another
program, 18-39
import, shapes, 18-7
inch mode format, (G70), 4-28
incremental
jog mode, 3-10
mode
center-angle arc, illustration, 7-17
change to, (G91), 4-29
move, execute, 3-11
positioning, 1-6
inequality operators, description,
19-26
initial move, parameter, 18-14
In-Position Mode
G64, cancel (G61), 4-21
modal, exact stop check, (G61), 4-11,
4-21
non-modal, exact stop check, (G9), 4-11,
4-21
IN-POST, program area label,
3-6
Ins (F3), 2-7
Insert (F8), 3-8
insert line, feature, 6-9
insert mode, 2-7
insert text
no overwrite, 6-5
overwrite, 6-6
inside profile, 5-38
inside profile, ramp moves,
illustration, 5-38
inside profile, ramp position,
illustration, 5-36
inspecting, programmed moves,
8-1
install
keyboard, 14-1
machine software, 14-1
RS-232 cable, 13-1
interface check, parameter,
18-12
introduction, 1-1
Index-11
CNC Programming and Operations Manual
P/N 70000487G - Index
IPM, defined, 4-30
irregular pocket
(M9367) correct tool diameter, from a
subprogram, 5-28
milling
(G169), 5-27
isometric spiral, illustration, 5-4
J
jog
:1, mode, 3-10
:10, mode, 3-10
:100, mode, 3-10
continuous, 3-7
conventional, 3-7
incremental move, execute, 3-11
mode
changing, 3-10
handwheel, to select, 3-13
modes, listed, table, 3-10
moves, description, 3-10
JOG - key, illustration, 3-4
jog and return. See jog/return
JOG key, illustration, 3-3
jog/return
description, 11-13
examples, 11-16
soft keys, listed, 11-14
jogging, machine (conventional),
3-11
join, colinear lines, 18-7, 18-39
K
keyboard
auxiliary, to display entity information,
17-7
description, 2-5
equivalent keypad keys, table, 14-2
external, 2-5
to install, 14-1
keypad
equivalent keyboard keys, table, 14-2
illustration, 2-2
keystrokes, retrieve, recorded,
6-12
L
labels, parameter, 18-26
large radius, mold rotation,
illustration, 5-51
Index-12
LENG, machine status display,
3-6
length offsets, ball end mill,
using, 9-12
length offsets, to measure, 9-6
LESS THAN operator,
description, 19-26
limit switch, 3-2
line segment endpoint definition
tools, illustration, 18-35
line segment tools, illustration,
18-34
line tools
description, 18-33
templates, listed, 18-44
linear interpolation (G1)
description, 4-4
illustration, 4-4
programming example, 4-4
LINES Help Template Menu,
parameters, table, 7-14
link or new shape, DXF
miscellaneous menu (F6),
description, 17-7
link test, screen data display, to
change, 13-6
link, testing, 13-7
list, program in another source,
10-14
loaded program, name, 3-6
loading, program for running,
10-3
local variables, description, 19-7
logging, to other drives, 10-6
logical symbols, listed, 19-25
logical terms, description, 19-25
loop
counter, 3-6
function, 5-66
programming
illustration, 5-66
LOOP - END, description, 19-23
LOOP, machine status display,
3-6
M
M, machine status display, 3-6
M00, program stop, 12-2
M01, optional program, 12-2
M02, 12-4
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Index
M02, program end, 12-2
M10, U-axis clamp, on, 12-2
M100, mirror image, 4-17, 12-3
M100, mirror image, canceled by
G92, 4-30
M1000, override, continuous
path parameter, 12-4
M105, dry-run, all axes, 12-3
M106, dry-run, NO Z-axis, 12-3
M107, disable, dry-run, 12-3
M107, dry-run OFF, 12-3
M11, U-axis clamp, off, 12-2
M19, 5-9
M19, spindle orientation, 12-2
M2, program end, 12-2
M20, disable feed hold, 12-2
M21, enable feed hold, 12-2
M3, spindle on forward, 12-2
M30, program end, 12-2
M4, spindle on reverse, 12-2
M40, 12-1
M41, 12-1
M42, 12-1
M43, 12-1
M44, 12-1
M5, spindle off, 12-2
M700, deactivate advanced
scaling, 12-3
M700, set advanced scaling,
12-3
M701, advanced scaling, 12-3
M8, coolant on, 12-2
M800, deactivate plane rotation
and set angle, 12-4
M801, activate plane rotation at
pre-set value, 12-4
M9, coolant off, 12-2
th
M900, activate 4 (U) axis
synchronization, 12-4
M901, deactivate 4th (U) axis
synchronization, 12-4
M9244, servo shut-off code,
12-4
M9351, clear, 12-4
M9367, correct tool diameter,
irregular pocket milling, 5-28
M9387, M-code, probe select,
19-21
M98, subprogram call, 12-3
M99, 4-24
All rights reserved. Subject to change without notice
17-April-04
M99, end subprogram, 5-65
M99, return from subprogram,
12-3
machine
home, return from, (G29), 4-16
home, return to, (G28), 4-15
position display, manual screen area, 3-5
setup, 3-1
setup, parameter, 18-14
software, DXF converter, 17-1
software, to install, 14-1
status display area, manual screen area,
3-5
status display, area labels, 3-6
machining
contour with many unknown intersections,
18-59
contour with many unknown intersections,
all tangent arcs, 18-61
milled pocket
X0 Y0 at center of radius, 18-67
X0 Y0 at the center of the large radius,
18-73
outside profile using contour, 18-55
outside profile with contour, 18-48
pocket milled into workpiece, 18-64
pocket milled into workpiece – X0 Y0 at
lower-left corner, 18-70
pocket, using contour and Drill, 18-77
series of holes, using Drill, 18-75
slot using contour, 18-52
macro
body structure, description, 19-13
defined, 19-8
G65 program, example, 19-15
G65 subprogram, example, 19-16
G66/G67 program, example, 19-16
letter addresses, listed, 19-14
passing, parameters, 19-14
programming (hole milling macro)
example, 19-18
setting, parameters, 19-14
SLOTMAC.G program, example, 19-17
string variables, description, 19-18
Main Edit Help Menu
description, 7-3
features, descriptions, 7-3
illustration, 7-4
managing, shape files, 18-47
Index-13
CNC Programming and Operations Manual
P/N 70000487G - Index
manual
machines, tool changes, to output, 18-30
mode
feed, to activate, 3-8
jog, incremental move, 3-11
move types, 3-7
rapid, to activate, 3-8
screen, illustration, 3-5
settings, 3-7
soft keys, illustration, 3-7
operation, 3-1
panel
illustration, 3-2
keys, listed, 3-3
LEDs, 3-4
screen, 3-5
Manual (F4), 3-7
MANUAL (F4), 11-14
Manual Data Input. See MDI
MANUAL/AUTO/S.STEP,
program area label, 3-6
mark
all programs, 10-7
program, 10-6
marked block, description, 6-2
marking, program blocks, 6-3
matrix pattern, illustration, 5-14
maximize, program storage,
10-4
maximum, memory allocated
description, 15-2
to change, 15-2
MC_5003, default spindle
orientation angle, 5-9
M-code
control codes, description, 12-2
control codes, table, 12-2
controlled functions, table, 12-2
description, 12-1
entering, 7-34
function, description, 12-1
listing, 7-33
M9387, probe select, 19-21
type in, manual, 7-35
MDI
defined, 3-12, 11-1
manual mode, 3-7
to use, 3-12
measure, length offsets, 9-6
memory, maximum allocated
Index-14
description, 15-2
to change, 15-2
menus
ARCS Help Template Menu, 7-17
Block Operations, pop-up, 6-13
Contour Parameters Menu, 18-9
Display, pop-up, illustration, 8-9
Draw parameters, pop-up, 8-4
Drill Parameter Menus, illustration, 18-22
DRILL/TAP Help Template Menu, 7-29
Edit Help G-Code, 7-32
End N#, pop-up, 8-8
Help Template Menu, 7-8
Help Template Menu, illustration, 7-4
LINES Help Template Menu, 7-14
Main Edit Help Menu, 7-4
MULTIPLE Help Template Menu, 7-22
PATHS Help Template Menu, 7-28
PLUNGE POCKETING Help Template
Menu, 7-27
Pocket Parameter Menus, illustration,
18-16
POCKETING Help Template Menu, 7-26
pop-up, 2-6
RAD/CHAMFER Help Template Menu,
7-20
Setup, 14-1
Shape Edit Menu, 18-4
Software Options Menu, 3-1
Start N#, pop-up, 8-8
message
displayed, 2-8
error, displayed, 2-8
line, manual screen area, 3-5
priority, 2-8
storage, 2-8
Message (F1), 3-8
mill (sync-on), programming
example, 16-5, 16-6
milled pocket
X0 Y0 at center of radius, machining,
18-67
X0 Y0 at the center of the large radius,
18-73
milling cavities, 5-45
milling cores, 5-45
minus sign, address, example,
19-9
minutes to decimal, conversion
formula, 16-1
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Index
mirror image, (M100), 12-3
mirror image, (M100), canceled
by G92, 4-30
miscellaneous
(F6) soft keys, listed, 18-40
menu, DXF converter, F6, 17-6, 17-7
miscellaneous codes. See Mcodes
mm mode format, (G71), 4-28
modal corner
rounding/chamfering, (G59,
G60), 4-19
modal function, 3-7
modal G-codes
defined, 4-1
listed, table, 4-1
modifiers
description, 19-1
listed, 19-1
mold rotation, (G45), 5-45
MOTION (F7), description, 18-8
motion mode
defined, 11-1
Draw, 8-6
switch to single-step mode, 11-2
move
delete, 18-6
shape, 18-5
moves, with unknown endpoints,
programming, 7-13
MULTIPLE Help Template Menu
description, 7-21
parameters, table, 7-22
multiple move
combinations, allowed, 7-21
commands, 7-21
using Edit Help Menu, 7-22
N
negative radius value, 7-16
negative signs, 7-10
nesting subprograms, 5-62
new
program, creating, 10-2
shape, DXF miscellaneous menu (F6),
description, 17-7
No Parity, 13-3
non-modal G-codes
defined, 4-1
listed, table, 4-1
All rights reserved. Subject to change without notice
17-April-04
non-synchronous rotary,
description, 16-2
NOT operator, description, 19-26
notes, on geometry, 18-45
number of parts, counter, 11-11
number, program block, 6-13
O
OEM, common (global)
variables, macro numbers,
19-7
off-line
entity information, to display, 17-7
passwords, listed, 15-1
software
DXF converter, 17-1
installation, 15-1
to exit, 15-1
Windows, to install, 15-2
Windows, to run, 15-2
offset mode, direction change,
9-19
offsets
activate, via program, 9-24
tool page, entering, 9-6
one shot moves, 3-12
operating mode, current, 3-6
operator prompts, 2-7
operators, listed, functions, 19-4
optimize, hard drive, 10-15
optional entry fields, description,
7-10
optional, program stop, (M01),
12-2
order of execution, codes, 12-4
order of operations, 19-10
Other, list programs, 10-6
output format pop-up menu,
illustration, 17-18
outside profile
circular profile cycle, (G171), 5-36
ramp moves, illustration, 5-38
ramp position, illustration, 5-36
using contour, machining, 18-55
with contour, machining, 18-48
override, continuous path
parameter, (M1000), 12-4
OVERRIDE, machine status
display, 3-6
Index-15
CNC Programming and Operations Manual
P/N 70000487G - Index
P
P/N 70000490, 6000M CNC
Setup Utility Manual,
referenced, 3-14
P/N 70000557, Probing Cycles,
referenced, 19-21
page down, feature, 6-9
page up, feature, 6-9
Pan, command, 8-11
Pan, display function, 18-40
parameter register, description,
19-8
parameters
description, 19-8
protected, to access, 15-1
viewing, 8-4
parametric programming
description, 19-7
parenthesis, example, 19-9
parenthesis, example, 19-9
parity, to set, 13-3
Parms (F9), 8-1
part programs, display, 10-6
part zero
location, 1-2
setting, 1-5
to set, (G92), 4-30
Z-axis, 9-5
parts counter, CNC, description,
11-11
PARTS, machine status display,
3-6
passing, macro parameters,
19-14
passwords, off-line, listed, 15-1
path number, 18-27
PATHS Help Template Menu,
parameters, table, 7-28
paths, option, description, 18-27
pattern drill cycles, 5-13
P-code, M99, end subprogram,
5-65
peck drilling cycle, (G83), 5-7
pending, messages, 2-8
perimeter pattern, illustration,
5-14
pick program, feature, 6-15
plane
illustration, 1-7
selection, 1-7
Index-16
plane selection
(G17, G18, G19), 4-11
description, 1-7
illustration, 4-12
play keys, feature, 6-12
plunge circular pocket milling,
(G177), 5-43
PLUNGE POCKETING Help
Template Menu, parameters,
table, 7-27
plunge rectangular pocket
milling, (G178), 5-44
pocket
cycles, description, 5-16
description, 18-16
menus soft keys, listed, 18-20
milled in workpiece
machining, 18-64
X0Y0 at lower-left corner, 18-70
Parameter Menus, illustration, 18-16
Parameters 1 Menu, parameters, listed,
18-17
Parameters 2 Menu, parameters, listed,
18-18
using contour and Drill, machining, 18-77
with islands (G162)
CAM, pocket parameters pop-up menu,
18-83
description, 5-29
DXF, program example, 17-20
subroutines, example, 5-29
using CAM, 18-21, 18-82
using DXF, 17-18
POCKETING Help Template
Menu, parameters, table, 7-26
point tools, templates, listed,
18-43
polar coordinates
description, 1-5
illustration, 5-13
pop-up menus, 2-6
Block Operation, 6-13
CAM, pocket parameters, 18-83
Misc, 18-41
miscellaneous menu, DXF converter, F6,
17-6, 17-7
output format, 17-18
program listing, 17-19
S-EDIT, 18-6
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Index
position
display modes, listed, 11-4
display, Z-axis, 9-6
locating, illustration, 1-4
positions, defining, 1-4
positive radius value, 7-16
positive value, assumed, 7-10
POST (F8), description, 18-25,
18-27
POST Menu
illustration, 18-28
parameters, listed, 18-29
saving, parameter settings, 18-30
post processor, automatic tool
changes, to output, 18-30
powering
off, 3-1
on, 3-1
practice, examples, 18-85
precautions, general, 9-20
primary display area, manual
screen area, 3-5
print program, feature, 6-14
PRINT variable, description,
19-8
print, portion of program, 6-14
printing
programs, 10-9
programs, from another source, 10-13
probe
M9387, M-code, probe select, 19-21
move, (G31), 4-16, 19-21
Probing Cycles, P/N 70000557,
referenced, 19-21
profile, cut, use Contour, 18-8
program
acess, most recent used, 6-15
area, labels, 3-6
area, manual screen area, 3-5
block
cancel edits, 6-5
copy and delete, 6-11
copying, 6-11
deleting, 6-4
displaying, 10-5
Help Graphic Screens, use, 7-10
mark and save, 6-11
marking, 6-3
number, 6-13
paste, within program, 6-12
All rights reserved. Subject to change without notice
17-April-04
renumber, 6-13
unmarking, 6-3
block separators, description, 19-1
blocks, copy, 6-16
cancel, Draw, 8-3
copy, other directories, 10-12
copying, to floppy disk, 10-8
create, new program, 10-2
definition, 1-3
delete, groups, 10-7
delete, on another drive, 10-14
directory
access, CNC programs, 10-2
description, 10-1
display, changing, 10-2
illustration, 10-1
display, soft keys listed, 10-5
edit, in another directory, 10-15
editor
activating, 6-1
activating, from Draw Graphics, 6-1
activating, from Manual Screen, 6-1
activating, from Program Directory, 6-1
end
M02, 12-2
M2, 12-2
M30, 12-2
formats, list all, 10-2
fragment, checking disk, 10-9
fragments, 10-9
getting started, 1-2
halted, clearing, 11-5
list, in another source, 10-14
listing
description, 6-2
include comments, 6-17
open program, 6-15
listing pop-up menu, illustration, 17-19
loading, 10-3
management, description, 10-1
mark, 10-6
mark all, 10-7
multiple move, using Edit Help Menu,
7-22
name, 3-6
name, description, 6-2
names, choosing, 10-3
offsets, activate, 9-24
parameters pop-up menu, illustration,
18-83
Index-17
CNC Programming and Operations Manual
P/N 70000487G - Index
parts counter, description, 11-11
parts counter, illustration, 11-11
print, 6-14
print, portion, 6-14
printing, 10-9
printing, from another source, 10-13
program, copy, 6-16
rename, 10-8, 10-12
restore, 10-8
running, 11-1
running, one step at a time, 11-1
run-time timer, description, 11-11
scroll, feature, 6-9
select, for editing, 10-3
sending, description, 13-7
stop, (M00), 12-2
storage, maximize, 10-4
T-code, tool page offset, 9-8
timer, description, 11-11
timer, illustration, 11-11
to delete, 10-5
to list contents, 10-5
to receive, 13-7
tool path, general precautions, 9-20
undeleting, 10-8
unmark, 10-7
unmark all, 10-7
using real-time Draw, while running
programs, 11-6
viewing with Draw, 8-1
wildcards, using, 10-10
Program (F2), 3-7
PROGRAM, program area label,
3-6
programmed, hold, 3-6
programming
angular motion, example, 4-5
arcs, description, 7-15
axis rotation, examples, 4-26
block separators, description, 19-1
circular profile cycle, 5-36
concepts, 1-3
conventions, rotary/U-axis, 16-2
corner rounding/chamfering, example,
4-20
elbow milling cycle, 5-56
ellipse, illustration, 5-1
exact stop check, non-modal, G9, 4-11
examples
description, 16-3
Index-18
drill (sync-off), 16-4
mill (sync-on), 16-5, 16-6
expressions, description, 19-4
expressions, examples, 19-5
expressions, listed, 19-4
facing cycle, 5-34
functions, description, 19-4
functions, listed, 19-4
G41, example, 9-21
G42, example, 9-22
G-code, from listing, 7-31
loop, illustration, 5-66
modifiers, listed, 19-1
moves, with unknown endpoints, 7-13
parametric, description, 19-7
part’s edge, 9-9
rectangular profile cycle, 5-38
single moves, 3-12
straight-line, example, 4-4
subprogram, example, 5-64
subprogram, illustration, 5-63
subprogram, multiple parts, 5-65
system variables, listed, 19-6
thread mill cycle, 5-40
tool offset modification, example, 19-3
user variables
block skip, description, 19-7
common (global), description, 19-7
description, 19-7
local, description, 19-7
read only, description, 19-7
static (global), description, 19-7
variable, description, 19-7
project feature
remove, a radius, 18-38
restore, sharp corner, 18-38
Project feature, description, 18-6
projecting, line segments, 18-6
prompts, 3-5
prompts, operator, 2-7
protected parameters, to access,
15-1
protocol, to set, 13-4
Q
quill position, Z0, 9-5
Quit (SHIFT+F10), description,
18-31
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Index
R
R, hot key, 18-39, 18-47
RAD/CHAMFER Help Template
Menu, parameters, table, 7-20
radius, remove, 18-6
ramp move, 9-10
rapid move
speed, adjusting, 3-8
viewing, 8-5
rapid traverse (G0)
description, 4-3
illustration, 4-3
program blocks, 4-3
Rapid, mode, 3-10
read only variables, description,
19-7
real-time
Draw mode, 8-1
Draw, using while running programs, 11-6
mode, Draw screen, 11-6
receive area, to clear, 13-7
receive mode, data control
codes, to use, 13-9
receiving
display, to set, 13-8
operations, to hold, 13-8
program, 13-7
record keys, feature, 6-12
recover paths, soft key, 18-41
recover shapes, soft key, 18-41
rectangular
pocket milling, (G78), 5-25
profile cycle, (G172), 5-38
reference point
return from, (G29), 4-16
return to, G28, 4-15
remaining, seconds, 3-6
remove
a radius, 18-38
radius, 18-6
rename
program, 10-8
programs, 10-12
renumber, program block, 6-13
repeat command, feature, 6-13
repeat function, 5-66
repeat, G-code output, 18-29
required entry fields, description,
7-10
All rights reserved. Subject to change without notice
17-April-04
Reset Rotary at 360, parameter,
16-2
reset, after stop, 3-1
reseting, the servos, 3-1
resetting, the servos, 3-2
restart, Draw automatic, 8-7
restarting, a program, 11-2
restore
block, feature, 6-5
deleted blocks
description, 6-5
using editing pop-up menu, 6-5
using SHIFT soft key menu, 6-5
programs, 10-8
sharp corner, 18-38
sharp corners, 18-6
Resume (F2), 13-8
retrieve, recorded keystrokes,
6-12
RETURN (F6), 11-15
return from subprogram, (M99),
12-3
reverse, arc direction, 18-6,
18-38
reviewing, messages, 2-8
rotary
non-synchronous, description, 16-2
synchronous, description, 16-2
rotary axis
programming conventions, 16-2
programming, in absolute, 16-2
programming, in incremental, 16-2
rotating XY mold around Z,
illustration, 5-50
rotation
around X and Y axes
large radius, 5-51
small radius, 5-47
around Z-axis, 5-52
round, a corner, 18-37
RPM, machine status display,
3-6
RS-232 cable, 13-1
RS-232 communication
connector, illustration, 13-1
Run parameter, 8-7
running
DNC, 13-9
program, one step at a time, 11-1
programs, 11-1
Index-19
CNC Programming and Operations Manual
P/N 70000487G - Index
RUNNING, program area label,
3-6
S
S.Step (F5), 3-7
S.Step, Draw, 8-6
sample, CAM programs, 18-48
saving, edits, 6-4
saving, POST parameter
settings, 18-30
Scale, display function, 18-40
scale, Draw, display size, 8-9
Scaling (G72) Help Graphic
Screen, to access, 7-1
S-code, description, 12-1
S-code, function, description,
12-1
screen clutter, eliminate, 8-5
screen saver, description, 2-6
screens
Auto, illustration, 11-4
communication, illustration, 13-2
COMPENSATION Help Graphic Screen,
7-11
DNC, 13-10
Draw (real-time mode), 11-6
Draw, simulation mode, 8-2
edit, illustration, 6-2
Enlarged Position Display, illustration,
11-7
Help Graphic Screen, illustration, 7-6
manual mode, 3-5
Scaling (G72) Help Graphic Screen, 7-1
Single-Step/Motion, illustration, 11-2
system information, 10-4
system information, illustration, 10-10
Test Link, illustration, 13-6
scroll, feature, 6-9
search
for text, 6-6
for word, 6-6
SEARCH
to select, auto mode, starting block, 11-5
using to select, single-step mode, starting
block, 11-3
secondary soft keys, listed, 9-4
seconds to degrees, conversion
formula, 16-1
seconds, remaining, 3-6
S-EDIT (F3), description, 18-4
Index-20
segment, delete, at forward end
of shape, 18-39
selecting
axis, 3-10
communication port, 13-3
program for editing, 10-3
program for utilities, 10-3
send mode, data control codes,
to use, 13-9
sending, program, 13-7
series of holes, using Drill,
machining, 18-75
SERVO RESET key, illustration,
3-3
servos
disengage, 3-1
reactivating, 3-1
reset, 3-2
shut-off code, (M9244), 12-4
to activate, 3-2
setting
advanced scaling, (M700), 12-3
baud rate, 13-3
data bits, 13-4
data type, 13-5
macro parameters, 19-14
parity, 13-3
part zero, 1-5
protocol, 13-4
receiving display, 13-8
shift, DXF miscellaneous menu (F6),
description, 17-7
software, 13-4
software limits, (G22), 4-13
stop bits, 13-4
test link display modes, 13-6
transmission display, 13-8
variables, 19-9
SETUP (F9), description, 18-25
Setup Menu, 14-1
setup parameters, listed, 18-25
shape
CAM
extension, 17-11
to create, 17-21
to view, 17-21
chaining geometry elements, to create,
18-46
cursor, using, 18-32
delete, 18-38
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Index
delete, a move, 18-8
delete, segment at forward end, 18-39
details, view listing, 18-40
edit, soft keys, 18-37
editing tools, illustration, 18-33
files, managing, 18-47
import, 18-7
import, from another program, 18-39
in G-code programs, 18-48
join, collinear lines, 18-7
list, soft key, 18-40
number, 18-26
option, description, 18-26
pocket, description, 18-16
reversed, parameter, 18-12
to cope, 18-5
to create, 18-4
to delete, 17-3, 18-6
to move, 18-5
Shape (F2), CAM mode, soft
keys, listed, 18-3
Shape Edit Menu, description,
18-4
Shape number, parameter,
18-10
SHIFT + F10 (Exit), 3-8
short form addressing, table,
19-24
shutting down, CNC, 3-1
simulation
mode, Draw, 8-1
size
change, 8-11
double, 8-11
half, 8-11
single-step mode
auto mode, switch to, 11-3
defined, 11-1
Draw, 8-6
MOTION mode, 11-1
motion mode, switch to, 11-2
program, to run, 11-1
S.STEP mode, 11-1
starting block, select
using arrows, 11-3
using SEARCH, 11-3
single-step/motion screen, 11-2
slot using contour, machining,
18-52
All rights reserved. Subject to change without notice
17-April-04
SLOTMAC.G macro program,
example, 19-17
soft key
calc distance, description, 18-41
calibrate keys, change fixture offset, 4-18
CAM mode, listed, 18-3
CAM mode, Shape (F2) listed, 18-3
CAM mode, to activate, 18-2
contour screen, listed, 18-15
display program, listed, 10-5
DXF converter, descriptions, 17-6
edit help, listed, 7-7
editing keys, description, 6-2
geometry list, description, 18-40
jog/return, listed, 11-14
labels, 3-6
labels, description, 2-6, 6-2
manual mode, illustration, 3-7
miscellaneous (F6), listed, 18-40
pocket menus, listed, 18-20
recover paths, description, 18-41
recover shapes, description, 18-41
secondary, tool page, listed, 9-4
shapes list, description, 18-40
teach mode, listed, 11-8
tool page, listed, 9-4
software
basics, 2-6
exiting, off-line, 15-1
parameters, 13-1
setting, 13-4
Software Options Menu, 3-1
spindle
at end, parameter, 18-15
at start, parameter, 18-15
off, (M5), 12-2
on forward, (M3), 12-2
on reverse, (M4), 12-2
orientation, (M19), 12-2
override, 3-6
speed, 3-6
speed control, description, 12-1
speed, parameter, 18-15
sync, 5-8
SPINDLE FORWARD key,
illustration, 3-3
SPINDLE OFF key, illustration, 3-3
SPINDLE OVERRIDE switch,
illustration, 3-3
Index-21
CNC Programming and Operations Manual
P/N 70000487G - Index
key,
illustration, 3-3
spiral, (G6), 5-3
spot drilling cycle, (G81), 5-6
START key, illustration, 3-3
Start N#, parameter, 8-8
start of block, feature, 6-6
start of program, feature, 6-6
starting block, select
auto mode, using SEARCH, 11-5
single-step mode, using SEARCH, 11-3
using arrow keys, 11-5
using arrows, 11-3
starting point
effect on orientation, illustration, 5-58
effect on size, illustration, 5-59
starting, Draw, 8-1
static (global) variables,
description, 19-7
status items, listed, 8-3
stepover
approach, 5-34
direction, 5-34
direction, parameter, 18-11
parameter, 18-10
value, 5-35
stop bits, to set, 13-4
stop, emergency, 3-1
storing, result of computation,
19-10
straight-line programming,
example, 4-4
string variables, description,
19-18
subdirectory, creating, 10-13
subprogram
addresses, 5-61
call, (M98), 12-3
description, 5-61
file inclusion, description, 19-26
loop, repetition, 5-62
M9367, correct tool diameter, irregular
pocket milling, 5-28
nesting, 5-62
orientation, illustration, 5-47
P-code, M99, end subprogram, 5-65
programming
example, 5-64
illustration, 5-63
multiple parts, 5-65
SPINDLE REVERSE
Index-22
specifics, illustration, 5-48
subroutines, pockets with
islands, example, 5-29
suppress, G-code output, 18-29
synchronous rotary, description,
16-2
system
information screen, illustration, 10-4
information, displaying, 10-10
variables, listed, 19-6
T
tapping canned cycle, (G84), 5-8
T-code, description, 9-4
T-code, tool page offset, 9-8
Teach (F5), 3-8
teach mode, 3-10
data, inputting, 11-9
description, 11-7
soft keys, listed, 11-8
to exit, 11-10
to start, 11-8
using, 11-10
template lettering conventions,
listed, 18-32
templates
arc, illustration, 18-36
circle tools, listed, 18-45
compensation help graphic, listed, 7-11
line segment endpoint definition,
illustration, 18-35
line segment, illustration, 18-34
line tools, listed, 18-44
point tools, listed, 18-43
test link
display modes, to set, 13-6
screen, to activate, 13-6
testing, data link, 13-5
testing, link, 13-7
text, deleting, 2-7
THEN, conditional statement,
19-22
thread mill cycle, (G181), 5-40
thread mill cycle, (G181), sample
program, 5-42
timer, CNC, description, 11-11
TIMER, machine status display,
3-6
All rights reserved. Subject to change without notice.
17-April-04
CNC Programming and Operations Manual
P/N 70000487G - Index
toggle endpoints, DXF
miscellaneous menu (F6),
description, 17-7
tool, 9-4
center, 9-9
change, parameter, 18-14
definition block, defined, 9-5
diameters, temporary change, 9-15
Draw, on or off, 8-4
edge, 9-9
management, description, 9-1
motion, tool compensation, 9-16
number, to find, 9-3
Tool (F9), 3-8
TOOL (F9), 11-15
tool compensation
acute angles, around, 9-18
cancel mode, (G40), 9-13
direction, change, 9-14
Draw, description, 8-5
tool motion, 9-16
Tool Compensation, parameter,
18-10
tool diameter
compensation
ball end mill, using, 9-12
left-hand, (G41), 9-9
plane you select, 1-7
right-hand, (G42), 9-10
correct for irregular pocket milling,
M9367, 5-28
parameter, 18-10
tool offset, modification
permanent, description, 19-2
permanent, format, 19-3
programming, example, 19-3
temporary, description, 19-2
temporary, format, 19-2
tool page
cursor, description, 2-7
definition, 9-1
diameter offset, 9-8
features, listed, 9-2
offsets, entering, 9-6
row, to clear, 9-3
single value, to adjust, 9-3
single value, to clear, 9-3
soft keys, listed, 9-4
soft keys, secondary, listed, 9-4
specific tool number, to find, 9-3
All rights reserved. Subject to change without notice
17-April-04
to activate, 9-1
tool-length offset, 9-5
using, 9-2
values, changing, 9-3
tool path
color, parameter, 18-12
compensation, (G41, G42), 9-9
to change, 18-8
to delete, 18-8
to generate, 18-8
TOOL, machine status display,
3-6
ToolComp, Draw, description,
8-5
tool-length offset, description,
9-5
tool-length offsets, setting, 9-7
top of contour, parameter, 18-11
top of pocket, description, 18-17
Total Blks Rec, 13-10
total free user space, 10-4
total space, available, system,
10-4
TPI/Lead, 5-8
transferring, variables, 19-9
transmission display, to set, 13-8
transmission operations, to hold,
13-8
transmit area, to clear, 13-7
troubleshooting, DXF converter,
17-5
truth table, logical symbols,
listed, 19-25
typeover mode, 2-7
typing in, address words, 7-34
U
U-axis
clamp, off (M11), 12-2
clamp, on (M10), 12-2
M900, example, 12-4
M901, example, 12-4
programming conventions, 16-2
programming, in absolute, 16-2
programming, in incremental, 16-2
unary minus, example, 19-9
unconditional LOOP repeat,
description, 19-23
undeleting, programs, 10-8
Index-23
CNC Programming and Operations Manual
P/N 70000487G - Index
unmark
a program, 10-7
all programs, 10-7
program blocks, 6-3
unsaved edits, canceling, 6-4
Use, Draw, description, 8-5
USER listing, 10-1
user macro G-codes, listed,
19-13
user macros, (G65, G66, G67)
description, 19-13
referenced, 4-22
user variables
block skip, description, 19-7
common (global), description, 19-7
description, 19-7
local, description, 19-7
read only, description, 19-7
static (global), description, 19-7
using, data control codes, 13-8
V
variable
direct transfer, 19-9
indirect transfer, 19-9
programming
description, 19-7
example 1, 19-11
example 2, 19-12
register, description, 19-8
setting, 19-9
view
listing of geometry elements, 18-46
listing of shape segment details, 18-40
programs with Draw, 8-1
View (F4) function, description,
18-7
W
warranty, iii
WHILE, conditional statement,
19-23
WHILE-DO-END, conditional
statement, 19-23
wildcard, (*), 10-11
wildcards, using, 10-10
Index-24
Window, display function, 18-40
window, sized, 8-10
Windows, off-line software
to install, 15-2
to run, 15-2
X
X0, Y0, Z0 Position, 1-4
X302, clear, 12-4
X-axis, description, 1-3
Xoff, 13-4
Xon, 13-4
XY
axis mold rotation, illustration, 5-46
location, defined, 18-29
mold rotations around Z, illustration, 5-50
passes, number of, parameter, 18-10
spiral view, illustration, 5-4
stepover, parameter, 18-10
Y
Y-axis, description, 1-4
Z
Z feedrate, parameter, 18-14
Z Location, description, 18-29
Z position, enter, manually, 9-8
Z step, parameter, 18-11
Z0, quill position, 9-5
Z-axis
description, 1-4
M801, example, 12-4
mold rotation, illustration, 5-52
move startup, 9-14
part zero, 9-5
position display, 9-6
rotation start & end angles, illustration,
5-53
rotation subprogram details, illustration,
5-53
zero degree reference, 1-6
Zero fill, description, 18-30
ZHOME (F3), 11-14
zoom in, Draw, 8-10
zoom, Draw window, 8-10
All rights reserved. Subject to change without notice.
17-April-04
U.S.A.
ANILAM
One Precision Way
Jamestown, NY 14701
(716) 661-1899
(716) 661-1884
anilaminc@anilam.com
ANILAM, CA
16312 Garfield Ave., Unit B
Paramount, CA 90723
(562) 408-3334
(562) 634-5459
anilamla@anilam.com
Dial “011” before each number when calling
from the U.S.A.
France
ANILAM S.A.R.L.
2 Ave de la Cristallerie
B.P. 68-92316
Serves Cedex, France
+33-1-46290061
+33-1-45072402
courrier@acu-rite.fr
Germany
ANILAM GmbH
Fraunhoferstrasse 1
D-83301 Traunreut
Germany
+49 8669 856110
+49 8669 850930
info@anilam.de
Italy
ANILAM Elettronica s.r.l.
10043 Orbassano
Strada Borgaretto 38
Torino, Italy
+39 011 900 2606
+39 011 900 2466
info@anilam.it
Taiwan
ANILAM, TW
No. 246 Chau-Fu Road
Taichung City 407
Taiwan, ROC
+886-4 225 87222
+886-4 225 87260
anilamtw@anilam.com
United Kingdom
ACI (UK) Limited
16 Plover Close, Interchange Park
Newport Pagnell
Buckinghamshire, MK16 9PS
England
+44 (0) 1908 514 500
+44 (0) 1908 610 111
sales@aciuk.co.uk
China
Acu-Rite Companies Inc.(Shanghai Representative Office)
Room 1986, Tower B
City Center of Shanghai
No. 100 Zunyi Lu Road
Chang Ning District
200051 Shanghai P.R.C.
+86 21 62370398
+86 21 62372320
china@anilam.com
P/N 70000487G
17-April-04
www.anilam.com
Download PDF