PCNC User Manual

PCNC User Manual
©2011 Tormach® LLC. All rights reserved.
Questions or comments?
Please email us at:
[email protected]
PCNC 1100 Series 3 Manual
Part Number 32397 – Rev C1-2
iiContents
Using Tormach PCNC 1100 Series 3
ii
32397 Rev C1-2
Contents
1.
Preface ............................................................................................. 1-1
1.1
1.1.1
1.1.2
1.1.3
1.1.4
1.2
Safety............................................................................................................................... 1-1
Electrical Safety................................................................................................................ 1-1
General Operating Safety .................................................................................................. 1-1
Safety Publications ........................................................................................................... 1-2
Safety Precautions............................................................................................................. 1-2
Personal CNC Concept ................................................................................................... 1-3
1.3
1.3.1
1.3.2
1.3.3
Performance Expectations .............................................................................................. 1-3
Cutting Ability.................................................................................................................. 1-3
Understanding Accuracy ................................................................................................... 1-4
Resolution, Accuracy and Repeatability of the PCNC ........................................................ 1-4
1.4
Scope and Intellectual Property...................................................................................... 1-4
1.5
Nomenclature .................................................................................................................. 1-5
2.
Preparation ...................................................................................... 2-1
2.1
2.1.1
2.1.2
2.1.3
2.1.4
Planning for Your PCNC ................................................................................................ 2-1
Electrical Connection ........................................................................................................ 2-1
Location and Mounting ..................................................................................................... 2-1
Computer Mounting Arrangement ..................................................................................... 2-3
Learning and Training....................................................................................................... 2-3
2.2.1
2.2.2
Receiving, Unpacking and Checking Shipment.............................................................. 2-4
Moving the Crate .............................................................................................................. 2-4
Uncrating and Inspection................................................................................................... 2-4
2.2
2.3
2.4
Assembling Y-axis Drive ................................................................................................. 2-4
Mounting the PCNC ....................................................................................................... 2-5
Lifting onto Stand ............................................................................................................. 2-5
2.4.1.1 Lifting from Below ................................................................................................ 2-5
2.4.1.2 Lifting from Above ................................................................................................ 2-6
2.4.2
Fixing to Stand ................................................................................................................. 2-6
2.4.3
Accessories ....................................................................................................................... 2-7
2.4.1
2.5
Power to the PCNC ......................................................................................................... 2-7
2.6
Power for Machine Accessories ...................................................................................... 2-7
2.7
Tormach Machine Controller and Software Installation ............................................... 2-8
Control Computer ............................................................................................................. 2-8
Setting Up Your Controller ............................................................................................... 2-8
2.7.2.1 Positioning the Controller....................................................................................... 2-8
2.7.2.2 Keyboard and Mouse ............................................................................................. 2-8
2.7.2.3 Display .................................................................................................................. 2-8
2.7.2.4 Speaker and Microphone Connections .................................................................... 2-9
2.7.2.5 Power Connections ................................................................................................ 2-9
2.7.3
Operating the Controller.................................................................................................... 2-9
2.7.3.1 About the Operating System ................................................................................... 2-9
2.7.3.2 Starting the controller ............................................................................................. 2-9
2.7.3.3 Stopping the controller ........................................................................................... 2-9
2.7.3.4 Mach3 License Installation ..................................................................................... 2-9
2.7.4
Machine Controller Maintenance and Configuration .......................................................... 2-9
2.7.4.1 Login and Software Installation .............................................................................. 2-9
2.7.1
2.7.2
iiContents
2.8
2.8.1
2.8.2
2.8.3
2.8.4
2.8.5
2.9
Connecting and Running the PCNC ............................................................................. 2-10
Main Switch and Control Panel ....................................................................................... 2-10
Changing the Spindle Speed Range ................................................................................. 2-12
Computer Control of the Spindle and Coolant.................................................................. 2-13
MDI for Entering G- and M-code Commands .................................................................. 2-14
Jogging the Axes............................................................................................................. 2-14
Summary ....................................................................................................................... 2-15
3.
Making Your First Part .................................................................... 3-1
3.1
3.1.1
3.2
Coordinates ..................................................................................................................... 3-1
Referencing the Machine................................................................................................... 3-1
Loading a Demonstration Program ................................................................................ 3-2
3.3
3.3.1
3.3.2
3.3.3
3.3.4
3.3.5
4.
Running the Demonstration Part-program .................................................................... 3-3
Part Material ..................................................................................................................... 3-3
Setting Work Offsets ......................................................................................................... 3-3
Cutting in Air.................................................................................................................... 3-4
Cutting the Actual Part ...................................................................................................... 3-4
Summary .......................................................................................................................... 3-6
Routes from an Idea to a Part ........................................................ 4-1
4.1
Controlling the PCNC..................................................................................................... 4-1
4.2
Choosing the Appropriate Design Software ................................................................... 4-2
4.3
4.3.1
4.3.2
4.3.3
4.3.4
4.3.5
4.4
Software for CAD/CAM ................................................................................................. 4-2
3D CAD ........................................................................................................................... 4-3
2D CAD ........................................................................................................................... 4-3
CAM ................................................................................................................................ 4-4
Running the G-code .......................................................................................................... 4-6
CAD/CAM Systems.......................................................................................................... 4-6
Programming with Wizards ........................................................................................... 4-9
4.4.1
Machining Wizard Concept ............................................................................................... 4-9
4.4.1.1 Selecting and Running a Wizard ............................................................................. 4-9
4.4.1.2 Standard Wizard Features....................................................................................... 4-9
4.4.1.3 G-code from a Wizard .......................................................................................... 4-10
4.4.1.4 Commercial Wizards............................................................................................ 4-10
5.
Machine Controls ............................................................................ 5-1
5.1
Machine Operation ......................................................................................................... 5-1
Operator’s Panel ............................................................................................................... 5-1
Tool Changing .................................................................................................................. 5-3
5.1.2.1 Tooling Strategy .................................................................................................... 5-3
5.1.2.2 Changing R8 Tools ................................................................................................ 5-3
5.1.2.3 Changing TTS Tools .............................................................................................. 5-4
5.1.3
Spindle Speed Ranges ....................................................................................................... 5-5
5.1.1
5.1.2
5.2
5.2.1
5.2.2
Screen Control Panels ..................................................................................................... 5-5
Using the Screens ............................................................................................................. 5-5
Families of Related Controls ............................................................................................. 5-5
5.2.2.1 Screen Switching Controls ..................................................................................... 5-5
5.2.2.2 Axis Control Family............................................................................................... 5-6
5.2.2.3 Jogging Control Family .......................................................................................... 5-7
5.2.2.4 Spindle Speed Control Family ................................................................................ 5-9
5.2.2.5 Feed Control Family .............................................................................................. 5-9
5.2.2.6 Program Running Control Family......................................................................... 5-10
5.2.2.7 Toolpath Control Family ...................................................................................... 5-11
Using Tormach PCNC 1100 Series 3
ii
32397 Rev C1-2
Contents
5.2.2.8 File Control Family .............................................................................................. 5-12
5.2.2.9 Work Offset and Tool Table Control Family......................................................... 5-12
5.2.2.10 MDI and Teach Control Family ............................................................................ 5-12
5.2.2.11 Loop Control Family ............................................................................................ 5-13
5.2.2.12 Modes and Mode Alarm Control Family............................................................... 5-13
5.2.2.13 Rotational Diameter Control Family ..................................................................... 5-14
5.2.2.14 Toolchange Position Control Family..................................................................... 5-14
5.2.2.15 Inhibits and Overrides Control Family .................................................................. 5-15
5.2.2.16 Feeds and Speeds Calculator ................................................................................ 5-15
5.2.2.17 Tapping Configuration Family.............................................................................. 5-15
5.2.2.18 Misc. Settings Control Family .............................................................................. 5-16
5.3
5.3.1
5.3.2
6.
USB Jogging Pendants .................................................................................................. 5-16
Jog/Shuttle Controller ..................................................................................................... 5-16
Keypad Pendant .............................................................................................................. 5-17
Using Multiple Tools ....................................................................... 6-1
6.1
6.2
Offsets and Coordinate Systems ..................................................................................... 6-1
Tool Length Offsets and the Tool Table ......................................................................... 6-1
Example Operation of Multiple Tools................................................................................ 6-1
6.2.1.1 To fill the table: ..................................................................................................... 6-2
6.2.1.2 Zeroing to work height ........................................................................................... 6-3
6.2.1.3 Using tool #2 ......................................................................................................... 6-4
6.2.1.4 Using other tools .................................................................................................... 6-4
6.2.1.5 Changing to a different work-piece ......................................................................... 6-4
6.2.2
How this multiple tooling setup works............................................................................... 6-4
6.2.3
Programming, Buttons, or Direct Entry ............................................................................. 6-5
6.2.1
6.3
Alternative Methods Setting Up Tools............................................................................ 6-6
Measuring techniques ....................................................................................................... 6-6
6.3.1.1 “Roll-Your-Own” Gauge Method ........................................................................... 6-7
6.3.1.2 Roller Gauge Method ............................................................................................. 6-7
6.3.1.3 Adjustable Parallel Method .................................................................................... 6-8
6.3.2
Comments on Accuracy .................................................................................................... 6-8
6.3.3
Working without the tool table .......................................................................................... 6-8
6.3.3.1 Direct Entry to Axis DRO ...................................................................................... 6-9
6.3.3.2 Using the Touch Buttons ........................................................................................ 6-9
6.3.4
Tool Table with General Tooling..................................................................................... 6-10
6.3.5
Tool table with the Tool Setter ........................................................................................ 6-10
6.3.1
6.4
Comments on Tool Offsets ............................................................................................ 6-10
6.5
Setting X and Y Offsets................................................................................................. 6-11
By eye ............................................................................................................................ 6-11
With a Probe ................................................................................................................... 6-11
Measuring Off an Edge ................................................................................................... 6-11
Laser Centering Techniques ............................................................................................ 6-12
6.5.1
6.5.2
6.5.3
6.5.4
6.6
How Work Offsets work ............................................................................................... 6-12
6.7
6.7.1
6.7.2
Multiple Work Origins ................................................................................................. 6-14
G54 Work Offset ............................................................................................................ 6-14
Other Work Offsets ......................................................................................................... 6-14
6.8.1
6.8.2
6.8.3
6.8.4
6.8.5
6.8.6
Cutter Diameter Compensation .................................................................................... 6-15
CAD/CAM and Wizards ................................................................................................. 6-15
Concepts for Cutter Diameter/Radius Compensation........................................................ 6-15
Caveats in the Use of Cutter Compensation ..................................................................... 6-15
Examples of Operation .................................................................................................... 6-16
Look Ahead Issues .......................................................................................................... 6-19
Other Restrictions ........................................................................................................... 6-21
6.8
32397 Rev C1-2
iii
Using Tormach PCNC 1100 Series 3
ivContents
6.8.7
6.8.8
7.
Perspective on Cutter Compensation ............................................................................... 6-21
Resources for Debugging Cutter Compensation ............................................................... 6-21
Part-programming Language Reference ....................................... 7-1
7.1
7.1.1
7.1.2
7.1.3
7.1.4
7.1.5
7.1.6
7.1.7
7.1.8
7.1.9
7.1.10
7.1.11
7.1.12
7.1.13
7.1.14
7.1.15
Definitions ....................................................................................................................... 7-1
Control Software............................................................................................................... 7-1
Linear Axes ...................................................................................................................... 7-1
Rotational Axes ................................................................................................................ 7-1
Scaling Input..................................................................................................................... 7-1
Controlled Point................................................................................................................ 7-2
Coordinated Linear Motion ............................................................................................... 7-2
Feed Rate.......................................................................................................................... 7-2
Arc Motion ....................................................................................................................... 7-2
Coolant ............................................................................................................................. 7-3
Dwell................................................................................................................................ 7-3
Units................................................................................................................................. 7-3
Current Position ................................................................................................................ 7-3
Selected Plane................................................................................................................... 7-3
Tool Table ........................................................................................................................ 7-3
Path Control Modes .......................................................................................................... 7-3
7.2.1
7.2.2
7.2.3
Interpreter Interaction with Controls ............................................................................ 7-4
Feed and Speed Override controls ..................................................................................... 7-4
Block Delete Control ........................................................................................................ 7-4
Optional Program Stop Control ......................................................................................... 7-4
7.2
7.3
Tool File .......................................................................................................................... 7-4
7.4
7.4.1
7.4.2
7.4.3
7.5
Part-programs Language ................................................................................................ 7-4
Overview .......................................................................................................................... 7-4
Parameters ........................................................................................................................ 7-5
Coordinate Systems .......................................................................................................... 7-5
Formatting Code Lines (Block) ...................................................................................... 7-5
Line Number..................................................................................................................... 7-7
Subroutine Labels ............................................................................................................. 7-7
Word ................................................................................................................................ 7-7
7.5.3.1 Number.................................................................................................................. 7-7
7.5.3.2 Parameter Value..................................................................................................... 7-7
7.5.3.3 Expressions and Binary Operations ........................................................................ 7-8
7.5.3.4 Unary Operation Value .......................................................................................... 7-8
7.5.4
Parameter Setting .............................................................................................................. 7-8
7.5.5
Comments and Messages .................................................................................................. 7-9
7.5.6
Item Repeats ..................................................................................................................... 7-9
7.5.7
Item Order ........................................................................................................................ 7-9
7.5.8
Commands and Machine Modes ...................................................................................... 7-10
7.5.1
7.5.2
7.5.3
7.6
7.7
Modal Groups ............................................................................................................... 7-10
G-codes .......................................................................................................................... 7-11
Rapid Linear Motion – G00............................................................................................. 7-13
Linear Motion at Feed Rate – G01................................................................................... 7-13
Arc at Feed Rate – G02 and G03 ..................................................................................... 7-15
7.7.3.1 Radius Format Arc ............................................................................................... 7-15
7.7.3.2 Center Format Arc ............................................................................................... 7-16
7.7.4
Dwell – G04 ................................................................................................................... 7-17
7.7.5
Coordinate System Data Tool and Work Offset Tables – G10 .......................................... 7-18
7.7.6
Clockwise/Counterclockwise Circular Pocket – G12 and G13.......................................... 7-18
7.7.7
Exit and Enter Polar Mode – G15 and G16 ...................................................................... 7-18
7.7.8
Plane Selection – G17, G18 and G19............................................................................... 7-19
7.7.9
Length Units – G20 and G21........................................................................................... 7-19
7.7.10 Return to Home – G28 and G30 ...................................................................................... 7-20
7.7.1
7.7.2
7.7.3
Using Tormach PCNC 1100 Series 3
iv
32397 Rev C1-2
Contents
7.7.11 Reference Axes – G28.1.................................................................................................. 7-20
7.7.12 Straight Probe – G31....................................................................................................... 7-20
7.7.12.1 Straight Probe Command ..................................................................................... 7-20
7.7.12.2 Using the Straight Probe Command ...................................................................... 7-21
7.7.12.3 Example Code...................................................................................................... 7-21
7.7.13 Cutter Radius Compensation – G40, G41 and G42 .......................................................... 7-22
7.7.14 Tool Length Offsets – G43, G44 and G49 ....................................................................... 7-23
7.7.15 Scale Factors – G50 and G51 .......................................................................................... 7-23
7.7.16 Temporary Coordinate System Offset – G52 ................................................................... 7-24
7.7.17 Move in Absolute Coordinates – G53 .............................................................................. 7-24
7.7.18 Select Work Offset Coordinate System – G54 to G59 & G59 P~...................................... 7-24
7.7.19 Set Path Control Mode – G61 and G64 ............................................................................ 7-25
7.7.20 Coordinate system rotation – G68 and G69...................................................................... 7-25
7.7.21 Canned Cycle – High Speed Peck Drill – G73 ................................................................. 7-26
7.7.22 Cancel Modal Motion – G80 ........................................................................................... 7-26
7.7.23 Canned Cycles – G81 to G89 .......................................................................................... 7-26
7.7.23.1 Preliminary and In-Between Motion ..................................................................... 7-28
7.7.23.2 G81 Cycle ............................................................................................................ 7-28
7.7.23.3 G82 Cycle ............................................................................................................ 7-29
7.7.23.4 G83 Cycle ............................................................................................................ 7-29
7.7.23.5 G85 Cycle ............................................................................................................ 7-30
7.7.23.6 G86 Cycle ............................................................................................................ 7-30
7.7.23.7 G88 Cycle ............................................................................................................ 7-30
7.7.23.8 G89 Cycle ............................................................................................................ 7-30
7.7.24 Distance Mode – G90 and G91........................................................................................ 7-30
7.7.25 G92 Offsets – G92, G92.1, G92.2 and G92.3 ................................................................... 7-31
7.7.26 Feed Rate Mode – G93, G94 and G95 ............................................................................. 7-31
7.7.27 Canned Cycle Return Level – G98 and G99 .................................................................... 7-32
7.8
7.8.1
7.8.2
7.8.3
7.8.4
7.8.5
7.8.6
7.8.7
7.8.8
Built-in M-codes ........................................................................................................... 7-32
Program Stopping and Ending – M0, M1, M2 and M30 ................................................... 7-32
Spindle Control – M3, M4 and M5 .................................................................................. 7-33
Tool change – M6 ........................................................................................................... 7-33
Coolant Control – M7, M8 and M9 ................................................................................. 7-34
Re-run from First Line – M47 ......................................................................................... 7-34
Override Control – M48 and M49 ................................................................................... 7-34
Call Subroutine – M98 .................................................................................................... 7-34
Return from Subroutine – M99........................................................................................ 7-34
7.9.1
7.9.2
7.9.3
Application Defined M-codes........................................................................................ 7-35
Self-reversing Tapping Cycles......................................................................................... 7-35
Goto Toolchange Position – M998 .................................................................................. 7-35
User Defined M-codes .................................................................................................... 7-35
7.9
7.10
7.10.1
7.10.2
7.10.3
Other Input Codes ........................................................................................................ 7-36
Feed Rate – F.................................................................................................................. 7-36
Spindle Speed – S ........................................................................................................... 7-36
Select Tool – T ............................................................................................................... 7-36
7.11
Order of Execution ....................................................................................................... 7-37
7.12
Error Handling ............................................................................................................. 7-37
8.
Machine Upgrades and Configuration........................................... 8-1
8.1
Fourth Axis – Rotary Table ............................................................................................ 8-1
Installing the Electronics ................................................................................................... 8-1
Utilizing the Fourth Axis................................................................................................... 8-1
8.1.2.1 Referencing and Zeroing the Fourth Axis ............................................................... 8-1
8.1.2.2 Diameter Compensation Feature ............................................................................. 8-1
8.1.3
Fourth Axis Applications .................................................................................................. 8-2
8.1.3.1 Engraving on a Periphery of a Cylinder .................................................................. 8-2
8.1.1
8.1.2
32397 Rev C1-2
v
Using Tormach PCNC 1100 Series 3
viContents
8.1.3.2
8.2
Gear Cutting .......................................................................................................... 8-3
Probes (Active and Passive) and Tool Setters................................................................. 8-4
Introduction to Uses of Probes and Tool Setters ................................................................. 8-4
Probing for Work/Tool Setting .......................................................................................... 8-5
8.2.2.1 Simple X/Y Probing ............................................................................................... 8-5
8.2.2.2 Z Probing............................................................................................................... 8-7
8.2.2.3 Comprehensive X/Y Probing .................................................................................. 8-9
8.2.2.4 Probe Calibration ................................................................................................. 8-12
8.2.3
Digitizing parts from a model or for reverse engineering.................................................. 8-13
8.2.4
The Probe Electrical Interface ......................................................................................... 8-13
8.2.5
Other .............................................................................................................................. 8-14
8.2.1
8.2.2
8.3
Auto-reverse tapping .................................................................................................... 8-14
9.
Warranty, Specifications, Customization and Troubleshooting . 9-1
9.1
Intended Use Statement .................................................................................................. 9-1
9.2
Support............................................................................................................................ 9-1
This manual – ALWAYS the first place to check!! ................................................. 9-1
Related documents found at: http://www.tormach.com/documents.html .................. 9-1
Our website at: www.tormach.com ......................................................................... 9-1
Email to: [email protected].................................. 9-1
Telephone Tormach at: 608-849-8381 .................................................................... 9-1
Fax Tormach at: 209-885-4534............................................................................... 9-1
•
•
•
•
•
•
9.3
Outside of the Scope of Intended Use ............................................................................. 9-1
9.4
Specifications................................................................................................................... 9-2
Mechanical ....................................................................................................................... 9-2
Electrical .......................................................................................................................... 9-2
System .............................................................................................................................. 9-3
Options ............................................................................................................................. 9-3
9.4.1
9.4.2
9.4.3
9.4.4
9.5
Maintenance .................................................................................................................... 9-3
Foreword – Understanding Machine Design ...................................................................... 9-3
9.5.1.1 Machine Stiffness................................................................................................... 9-3
9.5.1.2 Backlash, Friction, and Lost Motion ....................................................................... 9-4
9.5.1.3 Factors Combine .................................................................................................... 9-4
9.5.1.4 Adjusting Geometry ............................................................................................... 9-4
9.5.1.5 Achieving Accuracy in Machining.......................................................................... 9-5
9.5.2
Protecting from Rust ......................................................................................................... 9-5
9.5.3
Gibs, Dovetail Slideways and Lubrication ......................................................................... 9-5
9.5.4
Way Covers ...................................................................................................................... 9-6
9.5.5
Axis Gib Adjustment ........................................................................................................ 9-6
9.5.6
Adjusting Ballscrew Preload ............................................................................................. 9-8
9.5.6.1 Understanding Preloaded Angular Contact Bearings ............................................... 9-9
9.5.6.2 Making the Adjustment .......................................................................................... 9-9
9.5.7
Adjusting Mating Surfaces .............................................................................................. 9-11
9.5.8
Speed Calibration............................................................................................................ 9-11
9.5.9
Using a Non-standard Printer Port ................................................................................... 9-13
9.5.10 Defining Your Own Sizes for Step-mode Jogging............................................................ 9-14
9.5.11 Defining Probe Type ....................................................................................................... 9-15
9.5.12 Enabling 4th axis homing ................................................................................................ 9-15
9.5.13 Configuring to start in Metric units.................................................................................. 9-15
9.5.1
9.6
9.6.1
9.6.2
9.6.3
Troubleshooting ............................................................................................................ 9-16
Overview ........................................................................................................................ 9-16
Philosophy of Troubleshooting........................................................................................ 9-16
Tips and Tools for Troubleshooting (Equipment and Procedures)..................................... 9-19
9.6.3.1 Safety .................................................................................................................. 9-19
9.6.3.2 Tip on Computer Diagnostics ............................................................................... 9-19
Using Tormach PCNC 1100 Series 3
vi
32397 Rev C1-2
Contents
9.6.3.3 Tools ................................................................................................................... 9-20
9.6.3.4 Using the digital multi meter for electrical tests .................................................... 9-20
9.6.3.5 Contacting Technical Support............................................................................... 9-21
9.6.4
Frequently Found Problems (Repeat Offenders) .............................................................. 9-21
9.6.4.1 Loose Wires ......................................................................................................... 9-21
9.6.4.2 Wire Hairs ........................................................................................................... 9-22
9.6.4.3 Poor Cable Connections ....................................................................................... 9-22
9.6.4.4 Software Restart................................................................................................... 9-22
9.6.4.5 Sensors (on the PCNC the End of Travel Sensors) ................................................ 9-22
9.6.4.6 Flaky Computer ................................................................................................... 9-22
9.6.4.7 Control Software license not installed ................................................................... 9-22
9.6.4.8 Unexplained stop or limit switch error while running ............................................ 9-23
9.6.5
Which sub-system should I troubleshoot .......................................................................... 9-23
9.6.5.1 Computer and Coolant Power Distribution Sub-system ......................................... 9-24
9.6.5.2 Control Power Sub-system ................................................................................... 9-28
9.6.5.3 Computer Control Communication Sub-Section.................................................... 9-31
9.6.5.4 Axes Drive Sub-system ........................................................................................ 9-33
9.6.5.5 Spindle Drive Sub-system .................................................................................... 9-48
9.7
Mechanical maintenance............................................................................................... 9-56
9.8
Electrical maintenance .................................................................................................. 9-57
9.9
Preparation for Transport ............................................................................................ 9-57
9.10
Disassembly for Transport ........................................................................................... 9-58
10.
Appendices .................................................................................... 10-1
10.1
Appendix 1 – Not Used.................................................................................................. 10-1
10.2
Appendix 2 – Exploded Parts Views ............................................................................. 10-1
10.3
Appendix 3 - Use of a Standard PC to control PCNC ................................................ 10-14
10.3.1 Choice of computer ....................................................................................................... 10-14
10.3.2 Optimizing the Windows Installation............................................................................. 10-15
10.3.3 Installing the Control Software ...................................................................................... 10-15
10.3.3.1 Installing.............................................................................................................10-15
10.3.3.2 Vital Re-boot ......................................................................................................10-16
10.3.3.3 Testing the Installation ........................................................................................10-16
10.3.3.4 DriverTest After a Software Crash.......................................................................10-17
10.3.3.5 Manual Driver Installation and Un-installation.....................................................10-17
10.3.4 Optimization of Windows XP ....................................................................................... 10-18
10.3.4.1 Remove Unnecessary Services and Startup Programs...........................................10-19
10.3.4.2 Disable Power Management ................................................................................10-19
10.3.4.3 Disable sound card ..............................................................................................10-19
10.3.4.4 Disable Automatic Updates .................................................................................10-20
10.3.4.5 Set Computer to Standard PC not ACPI PC .........................................................10-20
10.4
11.
32397 Rev C1-2
Revision history........................................................................................................... 10-21
Index .................................................................................................. 23
vii
Using Tormach PCNC 1100 Series 3
Preface
1.
Preface
1.1
Safety
Any machine tool is potentially dangerous. Computer controlled machines are potentially more
dangerous than manual ones because, for example, a computer is quite prepared to plunge a 3"
diameter facing cutter at 50 inches per minute into a block of high-carbon steel or to mill the
clamps off your table.
The PCNC 1100 can deliver sufficient force to break brittle tools, to crush bones and to tear
flesh.
This manual tries to give you guidance on safety precautions and techniques but because we do
not know the details of your workshop or other local conditions we can accept no responsibility
for the performance of the machine or any damage or injury caused by its use. It is your
responsibility to ensure that you understand the implications of what you are doing and to
comply with any legislation and codes of practice applicable to your country or state.
1.1.1
Electrical Safety
Dual Power Input: The PCNC 1100 has two electrical power inputs. The primary supply is
230 VAC and is used for all axis and spindle motion. The secondary supply is 115 VAC. The
secondary supply is used to provide power to the accessory outlets only and is not used for
machine control. Either power supply can provide lethal electrical shocks. Both power inputs
should be unplugged before working in the electrical cabinet.
Grounding: Both primary and secondary power inputs must be grounded. During installation it
is not enough to assume that the ground line of a wall outlet is properly grounded. Check
continuity between the machine frame and true earth ground (water pipe or similar) to ensure a
good ground connection.
A Ground Fault Interrupt or GFI (i.e., Residual Current Circuit Breaker or RCCB in Europe)
outlet must be used to supply the power to the 115 VAC power input. Your computer, monitor
and coolant system are not bolted to the machine frame so proper grounding cannot be
assumed. The combination of electrical power and water based coolant systems makes the GFI
protection very important.
Electrical Panel: NEVER operate the machine tool with the cabinet door open. NEVER allow
a coolant pump to operate with the cabinet door open. DO NOT allow the coolant system to
flow coolant directly at the cabinet door seal or on the operator console controls. Neither the
cabinet door seal nor the electrical controls are sealed against liquids.
Retained Electrical Power: Electronic devices within the electrical cabinet may retain
dangerous electrical voltages after the power has been removed.
Electrical Service: Certain service and troubleshooting operations require access to the
electrical cabinet while the electrical power is on. Only qualified electrical technicians should
perform such operations.
1.1.2
General Operating Safety
Safe operation of the machine depends on its proper use and the precautions taken by each
operator.
Read and understand this manual. Be certain every operator understands the operation and
safety requirements of this machine before operating the machine.
Always wear safety glasses and safety shoes.
32397 Rev C1-2
1-1
Using Tormach PCNC 1100 Series 3
Preface
Always stop the spindle and check to ensure the CNC control is in the stop mode before
changing or adjusting the belt/pulley position, tool or work piece.
Never wear rings, watches, gloves, long sleeves, neckties, jewelry or other loose items when
operating or working around the machine. Long hair should be bound or kept under a hat.
Use adequate safeguarding around the operating envelope. It is the responsibility of the
employer to provide and ensure point of operation safeguarding per OSHA 1910.212 – Milling
Machine.
1.1.3
Safety Publications
Tormach recommends the following publications for assistance in enhancing the safe use of
this machine.
1.1.4
•
Safety Requirements for The Construction, Care and Use of Drilling, Milling and
Boring Machines (ANSI B11.8-1983). Available from The American National
Standards Institute, 1430 Broadway, New York, New York 10018.
•
Concepts and Techniques of Machine Safeguarding (OSHA Publication Number 3067).
Available from The Publication Office – O.S.H.A., U.S. Department of Labor, 200
Constitution Avenue, NW, Washington, DC 20210.
Safety Precautions
1. Do not run this machine without knowing the function of every control key, button, knob or
handle. Refer to the manual or contact Tormach if any function is not understood.
2. Protect your eyes. Wear approved safety glasses (with side shields) at all times. You should
never use compressed air to remove chips or to clean the machine. An air blast will often
launch a metal chip into a place it should not be.
3. Ear protection should be used on any operations that exceed sound levels of 85dBa.
4. Avoid moving parts. Before operating this machine remove all jewellery including watches
and rings, neckties and any loose-fitting clothing.
5. Keep your hair away from moving parts.
6. Take off gloves before you operate the machine. Gloves are easily caught in moving parts
or cutting tools.
7. Never operate with unbalanced tooling or spindle fixtures.
8. Remove all tools (wrenches, chuck keys, etc.) from the spindle and machine surface before
you begin. Loose items can become dangerous flying projectiles.
9. Use adequate work clamping. Do not allow your work piece to become a projectile.
10. Never operate a milling machine after consuming alcoholic beverages or taking strong
medication.
11. Protect your hands. Stop the machine spindle and ensure that the computer control is
stopped before you:
• Change tools;
•
Change parts or adjust the work piece;
•
Change the belt/pulley position;
•
Clear away chips, oil or coolant – always use a chip scraper or brush;
•
Make an adjustment to the part, fixture, coolant nozzle or take measurements;
•
Remove protective shields or safeguards – do not reach for the part, tool or fixture
around a guard.
12. Keep work area well lit. Ask for additional light if needed.
13. Keep the computer area clear of clutter. Recognize that machine motion can occur when
certain keys are pressed. Objects falling on the keyboard can result in unexpected motion.
14. Avoid getting pinched in places where the table, saddle or spindle head create “pinch
points” while in motion.
Using Tormach PCNC 1100 Series 3
1-2
32397 Rev C1-2
Preface
15. Securely clamp the work piece in a vise, on the table or in the fixture. Use proper holding
clamping attachments and position them clear of the toolpath. Be aware of larger pieces that
will be cut free during operations – loose parts can become projectiles.
16. Always use proper feeds and speeds, as well as depth and width of cut, to prevent tool
breakage.
17. Use proper cutting tools for the job.
18. Do not use dull or damaged cutting tools. They break easily and become dangerous
projectiles. Never use longer or larger tools than necessary.
19. Chips and dust from certain materials (e.g., magnesium) can be flammable. Fine dust from
normally non-flammable materials can be flammable or even explosive.
20. Chips and dust from certain materials can be toxic. Vapours from certain overheated
materials can be toxic. Always check a Materials Safety Data Sheet (MSDS) of suspect
materials. Refuse machining work requests of unknown materials.
21. If you are in any doubt you must seek guidance from a professionally qualified expert
rather than risk injury to yourself or to others.
1.2
Personal CNC Concept
The PCNC 1100 is a machine tool intended to make CNC machining more personal. As with
the evolution of personal computers, the evolution of personal CNC alters the paradigm of what
a machine tool is about. We aim for a machine tool so affordable that anyone can have one.
We feel that the work of engineers, inventors, technicians, hobbyists, educators and others will
be enhanced when they have access to CNC machinery. In education, each student can run his
own machine instead of waiting in line when the machine tool costs less than 20% of a small
machining center. In R & D, turn-around on prototype design takes minutes instead of days
when a machine is “at the ready” and on site. In general engineering, designs sent to the
production machine shop are improved when the design engineer has been more involved in the
prototype creation.
The PCNC offers the precision of a production machine but with cost/performance optimized
for short run operation.
1.3
Performance Expectations
1.3.1
Cutting Ability
The machine is capable of cutting most materials at or near their recommended feeds and
speeds. For example, for fast metal removal on 6061 aluminium we will run a 1/2" diameter 2
flute cutter at around 18 IPM (inches per minute) and 3000 RPM, using a full 1/2" depth of cut.;
that is a pretty good volumetric rate of metal removal so it is essential to clear chips with a
flood coolant. We will run smaller cutters when we are not trying to remove large amounts in a
hurry. For most aluminium work we use 3/8". The example above, using a 1/2" cutter, results in a
surface speed of 390 SFM (surface feed per minute), a 3/8" cutter needs 4000 RPM to get the
same surface speed, well within the performance envelope of the machine.
Cutting steel and iron needs a lower volumetric rate, thus slower feed and speed. The PCNC
will run best using smaller cutters when working with tougher materials. For example, the
general machining recommendation for some oil hardening steels is 30 SFM. Doing this with a
¾" end mill, the surface speed calculation indicates 150 RPM, but that is very near the
minimum spindle speed of the PCNC 1100 and certainly where limited power is available. By
switching to a 1/4" end mill the recommended spindle speed becomes 460 RPM, well within the
capability of the PCNC. By keeping close to general machining recommendations your tools
will last longer and you will have a better cut.
32397 Rev C1-2
1-3
Using Tormach PCNC 1100 Series 3
Preface
1.3.2
Understanding Accuracy
While a machine tool may seem absolutely rigid, the truth of the matter is that everything has
some elasticity. Related to elasticity is the compressibility of components such as ball nuts and
bearings. Preloading of bearings and ballscrews can remove the physical open space between
moving parts, but the technique cannot eliminate compressibility. The key to achieving
maximum accuracy is understanding and controlling the magnitude and direction of forces.
Maximum accuracy is achieved when the forces are minimized, as occurs in a finishing cut.
Maximum repeatability is achieved when the forces are repeatable, both in magnitude and
direction.
1.3.3
Resolution, Accuracy and Repeatability of the PCNC
The minimum discrete position move is 0.0001", this is the resolution of motion. Machine
accuracy is closely related to ballscrew accuracy. Our ballscrews are accurate to 0.0006" per
foot, but considering all the other factors that come into play, we prefer to keep accuracy
expectations to 0.0013" per foot. Repeatability will be better than 0.001" per foot.
Machining is a mix of science, skill and art. The caveat in stating accuracy and repeatability is
that these factors depend on the techniques used by the machinist. A skilled machinist can often
deliver accuracy that exceeds the accuracy specified by the machine builder, while an
inexperienced machinist may have difficulty delivering the expected accuracy. With this
understanding, we cannot tell you what accuracy you will be able to achieve in your own work.
Nevertheless, the accuracy specified by a machine builder remains an important reference
point.
1.4
Scope and Intellectual Property
This document is intended to provide sufficient information and detail to allow you to install,
setup and use your Tormach mill. It assumes that you have appropriate experience and/or
access to training for any Computer Aided Design/Manufacture software that you intend to use
with the machine. This document also assumes familiarity with typical Microsoft Windows
applications programs as the control software for the PCNC runs under the Windows operating
system.
Tormach LLC is dedicated to continual improvement of its products, so suggestions for
enhancements, corrections and clarifications will be gratefully received.
Tormach LLC, Art Fenerty and John Prentice assert their right to be identified as the authors of
this work. This work is copyrighted by Tormach LLC. The right to make copies of this manual
is granted solely for the purpose of training courses related to, evaluation of and/or use of the
PCNC. It is not permitted, under this right, for third parties to charge for copies of this manual
beyond the cost of printing.
Every effort has been made to make this manual as complete and as accurate as possible but no
warranty or fitness is claimed or implied. All information provided is on an “as is” basis. The
authors, publisher, and Tormach LLC shall not have any liability for, or responsibility to, any
person or entity for any reason for any loss or damage arising from the information contained in
this manual.
Tormach, PCNC1100 Personal CNC, PCNC770 Personal CNC, and Tormach Tooling System
are registered trademarks of Tormach. Windows XP and Windows 7 are registered trademarks
of Microsoft Corporation. If other trademarks are used in this manual, but not acknowledged,
please notify Tormach LLC so this can be remedied in subsequent editions.
Tormach milling machines and accessories are covered by one or more of the following U.S.
Patents: 7,386,362, D606,568, D612,406, D621,859 and Patent(s) Pending.
Using Tormach PCNC 1100 Series 3
1-4
32397 Rev C1-2
Preface
1.5
Nomenclature
This manual uses the following typographical nomenclature:
Software control
Refers to a Control Software “soft” control. (i.e., a Windows control on the PC screen).
Hardware Control
Refers to a physical button or switch on the Operator’s Panel of the machine.
G-code (e.g., G01X34.8)
Used to show G-code programs.
Key name (e.g., Enter)
Tells you to press the indicated key.
32397 Rev C1-2
1-5
Using Tormach PCNC 1100 Series 3
Preparation
2.
Preparation
This chapter describes the work required to unpack and to commission the
hardware and software of the PCNC.
It contains a lot of detail but can be completed in one or two hours by a person
familiar with CNC machines. Enough detail is given here so that a beginner
should be successful but some users may prefer to arrange for a machine tool
expert to do this work.
If your machine has already been set-up then you can skip this chapter
2.1
Planning for Your PCNC
2.1.1
Electrical Connection
The PCNC 1100 is shipped with a 3-wire cord and no electrical plug. There are several
different NEMA (National Electric Manufacturers Association) and non-NEMA plug patterns
that can be used. Straight blade patterns are common in household use; twist-lock patterns are
more common in industrial locations. Power required is 200 to 250 VAC, 50 or 60 Hz.
Continuous current is below 15 amps, but a 20 amp breaker or slow blow fuse is recommended.
Both primary and secondary power inputs must be grounded. During installation it is not
enough to assume that the ground line of a wall outlet is properly grounded. Check continuity
between the machine frame and true earth ground (water pipe or similar) to ensure a good
ground connection.
2.1.2
Location and Mounting
People experienced with CNC machining will undoubtedly have ideas as to how they want to
setup their PCNC (figure 2.1). While the machine can be configured in many different ways,
there are a few limitations. Many fully enclosed vertical machining centers incorporate high
volume coolant systems that make the inside of the machine look like the inside of a
dishwasher. The PCNC electrical
cabinet and operator console should
not be exposed to such conditions.
Additionally, there should never be
an enclosure or accessory that limits
access to the emergency stop. Please
keep these limitations in mind when
you plan your configuration.
If your prior experience is limited to
manual mills then keep in mind that,
as CNC dramatically extends your
machining capabilities, it will also
change the way you cut metal. When
your metal cutting is done by turning
handles on a manual mill your
operations will generally be limited to
cleaning up a surface, drilling a hole
pattern or cutting to a dimensional
Figure 2.1 – An example mounting on stand
outline. With manual milling many
people are accustomed to dry cutting, clearing chips with a small brush as they go.
32397 Rev C1-2
2-1
Using Tormach PCNC 1100 Series 3
Preparation
With CNC you have a whole new world open to you. In many cases you may turn the majority
of the stock into chips, cutting a shape out of a solid block of metal the way Michelangelo
would cut a sculpture from a block of marble. Unless you are limiting yourself to cutting cast
iron, wood, printed circuit boards or certain other materials, you will probably want a coolant
system on your machine. Mist coolant can be effective for keeping your cutting tools cool, but
it does little for clearing chips. Flood coolant will cool the cutting tools while clearing chips,
but is more challenging to contain. The table of the PCNC has drain slots and a hole tapped for
a pipe fitting to allow coolant collection, as is common on most small mills. Nevertheless, CNC
machining operations commonly produce so many chips that you simply cannot keep the table
drain running. At times, you may need a coolant flow that is simply too much for the table
drain. The little drain tray that is common under manual machines or the open frame setup of a
Bridgeport style knee mill just does not make it. We strongly recommend that you plan your
setup with a full motion tray, such that coolant will be captured as it overflows the machine
table within the full operating envelope of the machine.
Another reason to use a full motion tray is to reserve the space that will be required when the
machine moves. If you use a narrow drip tray or none at all, you should plan for full machine
motion plus some human space when you place the machine in your workshop. You do not
want to locate it where you can create crush points between the machine table and a wall. When
in operation, the X, Y and Z motions will not stop when they hit something. The machine will
move with hundreds of pounds of force, enough to punch through a wall, tip over the machine
or crush someone in the way.
Machine safety is the responsibility of the operator. This includes all aspects of safety: setup,
location, operation, security and all other factors that involve safety.
The PCNC requires a minimum plan area of 67" wide by 43" deep. This gives clearance for the
full motion of the table and for minimal access for cabling etc. The overall height required is
84" assuming that it is installed with the table at a working height of 36".
Tormach offers a range of stands, both ready-made and designs for you to have constructed
locally.
You should choose a well lit location and provide any additional task-lighting to make it easy to
setup work on the table.
Over time you will find that you accumulate a range of tools and tool holders so you should
allocate space for storage of these near the machine. A rack with numbered slots is convenient
5
USB jogging
pendant
4
LCD
Screen
6
Keyboard
3
2
1
Personal
computer
Personal
computer
Figure 2.2 – Computer and display
to avoid errors when doing tool changes during a job.
Using Tormach PCNC 1100 Series 3
2-2
32397 Rev C1-2
Preparation
2.1.3
Computer Mounting Arrangement
Keep the computer in a clean location, preferably inside the stand of the milling machine.
Resist the temptation to expose the computer in any way. Providing access to floppy disks, CDs
or direct computer controls will also open the computer to contamination and risk. Tormach
offers accessories that will allow you to operate the system without exposing your computer.
While there are many possible configurations for your machine control computer, we suggest
the following (figure 2.2):
1. USB bulkhead (panel mount) cable. This allows you to mount a USB socket directly on the
side of the cabinet. You can use a standard USB flash drive to transfer G-code programs
and other files to the machine controller. This is Tormach PN 30278 (USB bulkhead mount
cable – 3' Version 2.0 USB A to A extension M-F).
2. USB extension cable, extending the short cable normally found on keyboards and other
USB devices. Tormach PN 30279 (10FT USB 2.0 A to A Male/Female Extension Cable).
3. USB mini-keyboard. This is about the size of most laptop keyboards. The keyboard
includes a key which will power down the computer, allowing a convenient way to
shutdown the system. This is Tormach PN 31371 (Mini Keyboard). The keyboard can be
protected against coolant or chips by addition of Keyboard Cover PN 31384.
4. A Tormach USB jogging pendent is a very useful accessory for jogging, manual operations
and machine setup. Two options are available: a key based pendant (Tormach PN 30214
Pendent, 10 key USB keypad) and a jog/shuttle controller pendant that gives very fine
control of jogging speeds and distances. (Tormach PN 30616 Jog/Shuttle Controller).
5. LCD monitor signal cables are normally too short. Most inexpensive VGA signal extension
cables create serious signal degradation. This is particularly true with Super VGA screen
resolutions. Tormach PN 30280 (10FT SVGA Super VGA M/F Monitor Cable w/ ferrites)
is designed to extend Super VGA signals without degradation.
6. This is simply the AC power cord of the computer. The Computer switch on the operator
console controls a convenience outlet on the bottom of the machine control cabinet. If you
set the BIOS/CMOS configuration in your computer to start the computer when it sees AC
power then the console switch will allow you to start the computer from the console. You
should not shut off the computer from this switch due to issues with the Microsoft
Windows operating system, but you can turn the computer on from the keyboard/screen
controls.
There are several important points to bear in mind when using devices interfaced with USB
(Universal Serial Bus).
Do not attempt to run a G-code program that is stored on a USB drive (often called pen drives,
memory stocks, flash drives). Copy your G-code files into a folder on the hard drive (usually C:
of the control computer. Remove the USB drive after making the copy.
Do not use external USB hubs or devices like monitors or keyboards containing hubs.
USB devices can be affected by electrical noise on the computer mains power line. Devices
with large motors like compressors and ‘shop vacuum cleaners should not be plugged in to a
multiple outlet used by the control computer.
These rules minimize the chance of Windows deciding to manage USB devices when you are
running cuts on the mill.
The machine itself requires a 230 volt single phase wall power outlet rated at 6 amps, 13 amps
inrush. You should also provide a separate wall outlet for 115 or 230 volts, depending on your
locality, to act as power source for the computer, monitor and coolant pump (if used) which
should be specified to suit your local voltage.
2.1.4
Learning and Training
The final element of planning your installation is to consider the training that you and any other
users of the machine will need.
32397 Rev C1-2
2-3
Using Tormach PCNC 1100 Series 3
Preparation
This manual will give you the basic information required to start manufacturing components
with you PCNC. You must, however, expect to have to invest time in learning how to achieve
the best results. The areas which you will find easy and those which will require more effort
will of course depend on your background; you might be most comfortable with machining or
with component design or even with information technology.
We believe that you will find it highly cost-effective to acquire additional training materials for
areas of CAD/CAM/CNC which are new to you. Tormach sales can help point you in
appropriate directions.
2.2
Receiving, Unpacking and Checking Shipment
2.2.1
Moving the Crate
The PCNC is supplied on a standard pallet and
can be offloaded from a truck with a tailgate lift
and moved on smooth surfaces using a hydraulic
pallet jack. This makes delivery very economical
(figure 2.3).
Remove the crate top and sides with care as the
axis drive stepper motors are in vulnerable places
(figure 2.4).
The crated system weighs less than 1300 lbs (600
kg) nevertheless, it requires mechanical handling
to move it over rough ground and to lift it onto
the stand. Tormach advises you to employ the
services of a specialist rigger if the machine has to
be moved in situations where the pallet lifter cannot
be used or where there is no crane to lift the
machine onto its stand. It is possible to improvise
using a small trailer, a portable engine crane and
similar tools if there is no alternative but this risks
injury to you and damage to the machine.
2.2.2
Figure 2.3 – Crated machine as delivered
Uncrating and Inspection
After uncrating you should check the contents
against the parts listed on the packing slip and
inspect the machine for any damage incurred during
transit so any claims can be made within the
carrier’s deadline.
Figure 2.4 – Un-crated machine on pallet
2.3
Assembling Y-axis Drive
The PCNC is supplied with the Y-axis drive
motor mechanically disconnected. You are
advised to mount it before attempting to
remove the machine from its pallet.
•
Un-strap the stepper motor from its
transit position (figure 2.5).
•
Remove the sheet steel cover from the
Y-axis drive coupling box (at base of
column behind the machine).
•
Remove the four cap head screws
from the back face of the coupling
Using Tormach PCNC 1100 Series 3
Figure 2.5 – Y-axis motor as shipped and
mounting flange
2-4
32397 Rev C1-2
Preparation
box and loosen the two screws in the shaft coupling on the end of the Y- axis ballscrew
(4 mm or 5/32" hex wrench).
•
Use the cap screws to mount the motor on the back face of the coupling box. The wiring
runs downwards from the motor. It is important to ensure that the motor flange can pull
up flush to the machined face of the coupling box. Remove any paint that could cause
mis-alignment. After tightening the cap screws, back them off ¼ turn so the motor is
free to self align.
•
Ensure that the coupling is centrally positioned on motor shaft and the machined end of
the ballscrew and tighten the cap screws on the coupling. Then tighten the cap screws
holding the motor (figure 2.6).
•
Check that the axis turns with no tight
spots. The smooth (i.e., outside face) of
an old auto engine timing belt or polyvee auxiliary drive belt, which has been
cut to make a strip, can be used to turn
the coupling between the stepper motor
and ball screw (figure 2.9). If it does feel
tight then you need to recheck the
alignment of the coupling.
•
A final check of alignment should be
made when the machine is under
computer control. This involves
Figure 2.6 – coupling the Y drive motor
loosening the motor retaining screws ¼
turn and jogging the axis. The motor should show no signs of wobbling. If it does
wobble or move relative to the coupling housing then the coupling screws should be
slackened and retightened and the motor rechecked for movement. When alignment is
perfect, retighten the motor fixing screws and refit the coupling box cover.
2.4
Mounting the PCNC
2.4.1
Lifting onto Stand
The machine can be lifted onto an operating stand
by either of two methods: from below using the
base connection points or from above using a
slinging technique. In either case caution and
common sense are needed for the protection of the
machine and the people involved. Lifting up to1000
lbs can be simple with proper preparation and good
equipment, but it is never trivial and the dangers
involved should be taken seriously.
The work of lifting and placing heavy equipment is
called rigging. If you are not trained or prepared
then you should seek the advice of those who are.
Professional riggers can be found in most areas.
2.4.1.1
Lifting from Below
The base of the machine has four 7/8" holes. By
sliding two steel bars into these holes, at least 32" in
length, you end up with some outrigger wings that
can be used in combination with a fork lift truck to
lift the machine. These should be solid steel bars,
not pipes and be ¾" or 7/8" in diameter.
32397 Rev C1-2
2-5
Figure 2.7 – Hoist bar for slinging the
mill
Using Tormach PCNC 1100 Series 3
Preparation
2.4.1.2
Lifting from Above
The alternative way to mount your PCNC to a stand involves lifting from above. The eye in the
top of the column is suitable for lifting the machine, but it is not in line with the center of
gravity. The machine will tilt when lifted solely from the eye. The alternative is to sling the
machine using a combination of the eye and an eye in a T-nut on the table using a Tormach
special tool (part number 30576 - Machine Hoist Bar) (figure 2.7).
Figure 2.8 shows the geometry of the
slinging. The table should be as far away
from the column and as far to the right as
possible to optimize the balance.
It is most important that the machine is not
lifted by the control cabinet or by any of the
protruding stepper motors or the head or the
table. Incorrect rigging of the sling will
likely result in serious damage to the
PCNC.
The optimal balance for lifting should be
checked with the machine an inch or two
off the floor.
The X-, Y- and Z-axes can easily be moved
by hand if the covers on their coupling
boxes are removed. The smooth (i.e.,
outside face) of an old auto engine timing
belt or poly-vee auxiliary drive belt, which
has been cut to make a strip, can be used to
turn the coupling between the stepper motor
and ball screw (figure 2.9). As an
alternative to adjust the Y-axis to the front
position before you fit the stepper motor,
you can temporarily clamp a length of ½"
bar into the coupling and turn the bar with a
pair of slip-joint pliers (figure 2.10).
When you are ready to lift the machine you
should remove the nuts from the four
screws holding it down to the pallet.
2.4.2
Figure 2.8 – Slinging geometry
Fixing to Stand
Unlike very large mills, the level of
your mill does not significantly alter
machine accuracy. Leveling should
be sufficient to provide proper
coolant drainage, but precision
leveling is not necessary.
The supports under the corners of the
base of the mill are important to
Figure 2.9 – Manual moving table by back of old
machine accuracy. Despite the
toothed belt
apparent stiffness of the base casting,
it will respond to the weight of the machine. The result will be errors in the left/right tram of the
mill. For best accuracy, add shims under the left front or right front corners of the machine as
needed, such that the left/right tram is within your desired tolerance. Something like 0.002” is
usually all that is needed; however it is certainly possible to do even better.
Using Tormach PCNC 1100 Series 3
2-6
32397 Rev C1-2
Preparation
A welded steel stand is unlikely to be flat. Furthermore, if it is flat sitting on its own, it will sag
down as the 1300 lb machine is placed on it. Be aware that welded steel stands are neither stress
relieved nor as stiff as the machine base itself. If, for example, you place a 0.050” shim between
the base of the mill and the stand, you’re not actually lifting the corner of the base up by
0.050”. It is more likely that you are moving the mill up by 0.005” and the corresponding point
on the stand down by 0.045”.
2.4.3
Accessories
You should now try out the positioning of the screen, computer and coolant sub-system, if any.
2.5
Power to the PCNC
The PCNC 1100 is powered by 230 volt single phase AC (50 or 60 Hz). Auxiliary services like
the control computer and coolant are separate and can be 115 or 230 volts. Older coolant pumps
were supplied as 115 volt only. Later models can be configured to suit your auxiliary voltage.
Please note: The Tormach Machine Controller can be run on either 115 or 230 volts. For 230
volt applications, be sure to flip the switch in the back of the controller to "230". The Tormach
Coolant pump that comes with the Deluxe Stand is also dual voltage, but comes from the
factory wired for 115 volts. The user must remove the cover plate on the pump motor and
follow the wiring instructions inside the lid to reconfigure the pump motor for 230 volts. Other
products such as the Duality Lathe or companion high speed spindles are rated for 115 volts
only.
The main machine power lead is shipped in a protective tray. Terminate it with a suitable plug
for the wall outlet which you intend to use.
2.6
Power for Machine Accessories
There is an IEC inlet on the
bottom of the control cabinet
for the computer/coolant. This
should be connected to a GFI
(Ground Fault Interrupt) wall
outlet. This separate supply,
like the main machine supply,
is controlled by the main
power switch but allows use
of 115 volt accessories on a
230 volt mill.
The 115 VAC outlet under the
panel that is furthest from the
column feeds the coolant pump
Figure 2.11 – Power and interface connectors
and is controlled by the CNC
software. The pair of similar
outlets nearer the column is switched by the Computer switch on the front panel.
Both the 115 VAC power and ground are autonomous from the main machine power and
ground (230 VAC) in order to allow correct operation of the ground fault interrupter (GFI). The
computer control of the coolant outlet is accomplished by an isolated relay. Refer to the upper
portion of the circuit diagram in section 10.2 for details, wire numbers 200 through 207.
32397 Rev C1-2
2-7
Using Tormach PCNC 1100 Series 3
Preparation
2.7
Tormach Machine Controller and Software Installation
2.7.1
Control Computer
We recommend that you purchase a Tormach Machine Controller as part of the mill package as
the whole system will be covered by the Tormach warranty.
If, in exceptional circumstances, you wish to provide your own computer, it needs to run the 32
bit version (x86) of Microsoft Windows XP (Home or Professional edition) or Microsoft
Windows 7. Our experience is that the more modern and high performance the motherboard in
your computer is, the less reliable the performance running a real-time task will be. This is due
to many power saving and temperature control tricks used by the chip manufacturers. The
Tormach Machine Controller is specifically designed for real-time applications.
Details of the computer requirements and software installation for a standard PC can be found
in Appendix 3.
2.7.2
Setting Up Your Controller
2.7.2.1
Positioning the Controller
The controller should be positioned where it will remain
clean and dry. It can be placed vertically or horizontally.
When vertical it should be resting on the rubber pads.
When horizontal it should be resting such that the CDROM
drive is above, with the power button on the lower right
corner.
Do not allow anything to block the vented cabinet holes.
The steel cabinets design for PCNC series mills have
storage sections intended for the controller. The cabinet
storage areas are large enough to provide adequate cooling
without the need for additional fans. The controller remains
Figure 2.12 – Front of TMC
well protected in the machine stand, but access to the
controller is less inconvenient. This isn't a concern if you
power the controller through the computer outlet on the PCNC mill
(see the section below Operating the Controller: Starting the
Controller) and if you extend the USB ports using USB Bulkhead
Cable (PN 302781) which positions a USB port to the outside of the
machine stand.
2.7.2.2
Keyboard and Mouse
The controller supports with USB (figure 2.13 - sockets at 5) or
PS/2 style mouse and keyboard connections (sockets 1 & 2).
Wireless keyboards and mice are not recommended. Both powered
and passive USB hubs have a history of problems when used in
combination with Mach3 software. We recommend that all USB
devices plug directly into the USB ports on the controller (sockets 5).
2.7.2.3
Figure 2.13 – Rear of
TMC
Display
Connect the display to socket 4 - figure 2.13.
1
Refer to http://www.tormach.com/document_library/DS30278_USBBulkheadCable.pdf
Using Tormach PCNC 1100 Series 3
2-8
32397 Rev C1-2
Preparation
2.7.2.4
Speaker and Microphone Connections
Speaker and microphone connections are possible but not recommended.
2.7.2.5
Power Connections
Check the voltage setting before connecting power (figure 2.13 – location 13). The controller
can be set to run on either 115 VAC or 230 VAC and will operate equally well on 50 or 60 Hz
power.
2.7.3
Operating the Controller
2.7.3.1
About the Operating System
The MachOS operating system is built with Microsoft Embedded Standard, but it looks and acts
much like Windows XP Pro. If you are familiar with Windows XP, then you know how to use
MachOS. The Tormach Machine Controller has s been designed and configured to work with
Mach CNC control software. Under most circumstances, no modification to the configuration
is needed. Modification to the configuration of the operating system can disable the controller.
2.7.3.2
Starting the controller
The Controller is configured to boot immediately upon the application of power. This allows
you to turn on the computer using a remote power switch, such as the power switch marked
COMPUTER on the front of the PCNC mill control panel. You can also start the controller
using the power button on the front panel. For the present just power the Controller and your
monitor from a wall outlet.
PCNC control software (Mach3) will start immediately after the Controller boots. If you need
to exit the control program you can restart it using the desktop icon.
2.7.3.3
Stopping the controller
The controller should be stopped by clicking on the Start > Shutdown function on the lower left
corner of the computer screen. It is not a good idea to simply turn off the controller, it should
be allowed to shutdown properly.
After you have shutdown the computer, turn off the computer power using the switch on the
front panel of the mill. This will allow you to use the power switch to turn the computer back
on. If you forget to turn off the power then you will not be able to turn it on using a quick offon cycle of the computer power switch. The computer needs to be off for 30 seconds before the
function of "Boot upon Power" will work.
2.7.3.4
Mach3 License Installation
Note: The controller is shipped without the Mach3 license on its hard drive. The Mach3
control program installed, but without the license it will only work in demo mode (limit 500
lines of code) without the Mach3 license. Tormach ships the Mach3 software license on a
separate CD. To install you license file, simply insert the license CD after the controller has
booted up. The license file will automatically be transferred to the hard drive. You can then
remove the license CD and store it in a safe location.
2.7.4
Machine Controller Maintenance and Configuration
2.7.4.1
Login and Software Installation
The controller boots up to an automatic login with Username: Operator and a blank
password. The Operator has rights to use the software but cannot install software or modify the
MachOS configuration. If you need to install software or modify configuration you must
logout Operator and login again with:
32397 Rev C1-2
2-9
Using Tormach PCNC 1100 Series 3
Preparation
Username: Administrator
Password: administrator
Note that the upper/lower case is important. The Administrator login will be necessary if you
need to reinstall the PCNC software or install new software.
The controller is licensed as a dedicated machine controller. Do not attempt to use it as a
desktop computer and do not try to install general purpose software such as Microsoft Office or
Microsoft Word. You can install CNC related software such as CAD, CAM, or machining
utility programs such as Machinist's ToolBox although Tormach does not recommend this..
2.8
Connecting and Running the PCNC
You have now completed the installation and merely need to connect the PCNC to the
computer.
Now close down MachOS and switch off the Controller. Connect the parallel port of the
computer (figure 2.13 socket 11) to the D25 connector on the underside of the PCNC control
cabinet. The cable provided to connect the computer to the mill meets IEEE 1284
specifications. This provides a high level of immunity to electrical noise, which is important to
reliable operation. Do not use inferior cables.
Now power the Controller from the outlet near the D25 connector and if relevant, power the
monitor from the connector adjacent to it below the PCNC control cabinet. Viewed from
behind, the inlet is on the right next to two outlets for computer and monitor. The coolant pump
outlet is to the left of these (figure 2.11).
2.8.1
Main Switch and Control Panel
The rotary main switch on the right hand side of the control cabinet disconnects the mains
power from the PCNC itself and isolates computer/coolant (115/230 VAC) outlets that are on
the bottom of the cabinet.
Warning: You should not open the control cabinet until the mains power to the machine and to
the computer/coolant pump are both removed from the wall outlet. Live parts may be exposed
even when the main switch is in the off position.
Computer On/Off
Figure 2.14 – Operator’s Panel
Using Tormach PCNC 1100 Series 3
2-10
32397 Rev C1-2
Preparation
Warning: The following power-up and power-down sequences should be followed exactly to
avoid the risk of unintended machine motion which could cause injury to you or damage to the
machine.
Switch the main switch ON and switch the computer power on at the PCNC control panel
(figure 2.14).
The computer will power up and
run the Control Program (figure
2.15).
This will allow you to perform all
the important functions on the
standard machine. If you have the
4th axis or want to use G-code
features like Optional Stop then
you may wish to use the
Comprehensive Run screen
(figure 2.16). In this case click
the Comp Run button to change
the display.
The screen “Light Emitting
Diodes” (LEDs in this manual)
by the Reset button will be
flashing as will the Machine OK LED.
Figure 2.15 – Simple main screen
Now, returning to the operator’s panel:
Start and EStop
The Start button will energize the
circuits for the axis drives and for the
spindle motor. The Stop button stops all
motion and is the Emergency Stop
(EStop) control. The Stop button locks in
the off position once it has been pressed
as safety feature. It can be released by a
turning the button-head a quarter-turn
clockwise. Note: Once the stop button has
been pressed the start button is
inoperative until the stop button is
released.
Figure 2.16 – Comprehensive Run screen
The Machine LED indicates that the Start button has been pressed. When it is lit then the
Machine OK LED on the computer screen should be solid green. If this does not happen then
you should check that the cable between the PCNC and computer is fully plugged-in at both
ends. You will be able to test some controls on the PCNC, even if the LED does not give the
correct indication but you will have to find the fault before you can move the PCNC axes under
computer control.
Shut Down
1. Push the red Stop button (mentioned below)
2. Exit from Mach 3
3. Perform a soft shut down of the control computer (click the Windows Start button on the
screen, then select Turn Off Computer and the Turn Off)
4. Switch the Computer On/Off switch on the machine control panel to the Off position
32397 Rev C1-2
2-11
Using Tormach PCNC 1100 Series 3
Preparation
Note: You should not shut down or turn off the control computer while the PCNC mill is
powered up! Should this happen, the Z axis may drop damaging tools or causing injury.
Spindle
An important safety interlock is that the rotation of the spindle can be disabled (while
maintaining axis drive power) by the Spindle Lockout key-switch. The switch on the
spindle drive door performs the same function. These are used to ensure that the spindle cannot
start when an R8 tool holder is being changed (door open) or when a tool is being changed in a
collet chuck. Turning the Spindle Lockout key or opening the spindle cover while the
spindle is running will also stop the spindle. Stopping the spindle in that way will not damage
any components, but it is generally a poor practice.
The controls above the key-switch are all concerned with manual control of the spindle. If the
Manual/Auto switch is in the Auto position then none of the other spindle controls have any
effect. In the Manual position the computer control of the spindle is disabled.
Switch to Manual and turn the speed control knob fully counterclockwise. Press the Spindle
Start rocker. The spindle should start turning slowly in the clockwise (forward) or
counterclockwise (Reverse) direction (viewed from above) depending on the setting of the
Forward/Reverse switch. You can safely switch directions while the spindle is turning.
Try changing the speed using the rotary control knob. The actual speed will depend upon which
of the two pulley ratios you have selected.
Pressing the Spindle Stop rocker will halt the spindle.
Coolant
The Coolant switch controls the power to the coolant pump outlet on the underside of the
control cabinet. In the Off position the outlet is not powered and the pump will not run. In the
On position power is applied to the outlet and the pump will run until the switch is switched to
either off or auto positions. In the
Auto position outlet power is under
program control the pump will run if
the Control Program requests coolant.
Accessory Socket
The Accessory socket is for
connection of accessories such as a
touch probe. See Chapter 8 for details
of the interface.
2.8.2
Changing the Spindle Speed
Range
The PCNC has two speed ranges. The
low range, 100 to 2000 RPM, is
suitable for most machining
operations with ferrous and other
tough materials. The high range, 250
to 5140 RPM is suitable for small
Figure 2.17 – Changing spindle pulleys
diameter cutters, plastics and nonferrous materials. The range change
is performed by moving the V-belt from the upper pair of pulleys (high speed range) to the
lower pair (low speed range).
Open the spindle drive door. The interlock will prevent the motor from running. Note: Opening
the spindle drive door will also stop a running spindle; however, this is a safety hazard and
Using Tormach PCNC 1100 Series 3
2-12
32397 Rev C1-2
Preparation
should not be used as a substitute for stopping the spindle with
the spindle controls in the Control Software. Use the rear
handle to unlock the motor mounting plate and pull the motor
forwards. The belt will slacken and can be moved from one set
of pulleys to the other (figure 2.17).
For the following tests, select the low speed range by placing
the belt on the lower pair of pulleys). Retighten the belt so
there is between 1/8" and ¼" movement between the pulleys,
lock the motor mounting and stow the handles in the vertical
position.
Figure 2.18 – Spindle controls
2.8.3
Computer Control of the Spindle and Coolant
Switch the Spindle and Coolant to Auto on the control panel. Make sure the computer is
displaying the Simple Run screen as shown in figure 2.15. The
portion shown in figure 2.18 shows the controls for the
spindle.
Use the mouse to click the Hi/Lo button. You will see that the
screen LEDs depicting the pulleys will change and the
appropriate maximum speed will be displayed below them.
Choose the Low setting to correspond to the PCNC pulleys.
Note: Just after starting the system the screen LEDs may not
correspond to the indicated maximum speed. The speed value
is always correct and a click on the Hi/Lo button will bring the
LEDs into step.
Figure 2.19 – Setting S word
Next to the label S, is a digital read-out (DRO) of the
requested spindle speed. You can change this by clicking the
mouse on it. It will become highlighted. Type a number, say 500 (for 500 rpm) and press Enter.
Figure 2.19 shows the screen just before pressing Enter. If you make a mistake you can press
Esc to return to the original value.
This technique is used for setting any DRO. Remember to use Enter after any DRO change. If
you forget and just click on another DRO, then any value you have just entered will be
discarded. This is designed to avoid accidental changes.
Now check that the machine is safe and that the motor door is closed and click on the Spindle
CW F5 button. The spindle will start running. Clicking the button again will stop it.
The F5 in the caption tells you that function key F5 is a “shortcut” to this button; it can also be
used to start and stop the spindle.
Notice that there are two sets of screen LEDs. The outer set indicates that the machine is
dwelling to ensure the spindle has started and fully stopped. The center LED indicates that it is
running.
If you have connected a coolant pump to the outlet under the control box (see vacant outlet in
figure 2.10) then you will be able to control it by the Coolant Ctrl-C button or its shortcut which
is the Ctrl-C key.
Beware of the
position of the
coolant nozzle
before you try this!
Figure 2.20 – MDI Line in use
32397 Rev C1-2
2-13
Using Tormach PCNC 1100 Series 3
Preparation
2.8.4
MDI for Entering G- and M-code Commands
When you are making parts the commands to the machine (G- and M-codes) will generally be
read from a file. It is however often convenient to command the PCNC directly. This can be
done by typing command into the Manual Data Input (or MDI for short) line.
The command to start the spindle in the clockwise direction is M3 and the command to stop it is
M5.
Click the mouse in the bar marked MDI. It will highlight. You type the command in the
highlighted line. Unlike in DROs, the Backspace, Del, Left and Right arrow keys are available
to help you correct any typing errors.
When you press Enter the command will be executed. Pressing Esc abandons it and closes the
MDI line. You can try starting and stopping the spindle with M3 and M5 G-codes.
Notice that the recent commands are displayed in a fly-out box. You can choose one of these to
copy into the MDI line using the Up and Down arrow keys.
Figure 2.20 shows the MDI line after the spindle has been started (M3) and the M5 has been
typed but not yet executed by Enter.
There are some handy features of the MDI box. It can be
opened by pressing Enter (rather than needing a mouse
click). It stays open after a command has been executed.
It can be closed by Enter when it is blank.
Note: All keystrokes go to the MDI when it is open so it
is not possible to execute shortcuts or jog the axes. If the
keyboard does not do what you expect then you
probably still have the MDI line open.
Figure 2.21 – Simple jog controls
2.8.5
Jogging the Axes
The final thing to try before actually making your first part is to move (jog) the PCNC axes
using the keyboard.
There are several options for jogging which will be explained in detail below. The jogging
controls are at the top right hand side of the screen (figure 2.21).
Click the Jog ON/OFF button (or use its shortcut Ctrl-Alt-J) to turn on the screen LEDs beside
it if they are not already on. Click Jog Mode (or use its shortcut) to turn on the larger of the
LEDs above the word Cont (for Continuous jogging). Type the value 10 into the Slow Jog Rate
DRO; do not forget the Enter to accept the value)
In the next steps you may find the directions of movement are unexpected. Therefore, when you
use the arrow keys you should be prepared to quickly release the key if the axes moves in an
unexpected direction or is near its limit of travel. Now, press the Left, Right, Up and Down
arrows on the keyboard. The table will move while you hold the key down. If you crash into the
limit switches then the LED beside the red Reset button will flash and the machine will stop.
Click on Reset and very carefully jog the other way. Take care not to mechanically hit the limit
doing this in the wrong direction. You will lose the referenced status if you trip a limit switch.
You might find the directions of movement are unexpected. Figure 2.22 shows the tool above a
work piece. The positive X, Y and Z directions are marked by arrows. If you press the Right
arrow key then the tool will move in the positive X direction (i.e., to the right of the work).
Similarly the Up arrow moves the tool in the positive Y direction (i.e., towards the PCNC
column). Of course, this actually happens on the PCNC by the table moving under the tool but
you must imagine what it would look like if you were sitting on the table and watching the tool.
Using Tormach PCNC 1100 Series 3
2-14
32397 Rev C1-2
Preparation
You should jog around
until you are quite
confident which way the
machine moves when you
press any key. Notice that
the values in the Axis
DROs change as you jog
the tool around.
Jogging the Z-axis is done
by using the Page up and
Page down keys. Here of
course it is the tool that
moves, so “Up” is indeed
up.
Figure 2.22 – Jogging is to move the tool relative to work
2.9
Summary
This chapter has covered a lot of basic ground. Much of it only has to be done once. You may
however wish to revisit the latter parts if you are not fully confident with using buttons, DROs,
the MDI and jogging. We will give less detail on using these (e.g., assume you know about
shortcuts and when to use Enter) in subsequent chapters.
32397 Rev C1-2
2-15
Using Tormach PCNC 1100 Series 3
Making your first part
3.
Making Your First Part
This chapter shows you how to make your first part with the PCNC. It assumes
that you have no prior experience with running a part-program on a Computer
Numerically Controlled machine tool.
Even if you have previous experience you will find that following this tutorial
gives you an introduction to the controls of the machine.
3.1
Coordinates
Coordinates are simply how you describe where the tool is positioned. We assume that you
have the computer and PCNC setup and switched on and are looking at the Simple screen.
3.1.1
Referencing the Machine
You have seen that jogging the machine moves the tool and this changes the numbers in the X-,
Y- and Z-axis DROs. You may have wondered where these numbers come from and indeed
doubted that they are very sensible. The answer is that they are probably meaningless. The
computer has no way of knowing yet where the tool or table is positioned.
Referencing is the process which puts the
machine in a known mechanical position
and sets the corresponding axis DROs.
The known position is where the limit
switches operate with Z at the top of the
column and the spindle over the top lefthand corner of the table. This position is
called Home and so these limit switches
are called the Home switches. Their
operation is very obvious on the Z-axis. A
software trick makes the X and Y
arrangement slightly harder to understand
but this is of no importance at present.
Figure 3.1 – The axis DROS un-referenced
Figure 3.1 shows how the DROs might look when you start up the system. They have arbitrary
values in them and the three screen LEDs are red.
Check that the LEDs by the red Reset button are not flashing and that nothing is in the way of
movement of the table and head of the
PCNC. Click the Ref All button.
The Z-axis will first move up to the top of
the column, stop at the switch and then
move down a fraction. The Z DRO will be
set to zero and its LED turn to green. This
will be followed by the same action with X
and Y. Be wary the first time you do this
and if an axis does not stop at its switch
you must hit the EStop button on the
PCNC control panel and look at the
Maintenance/Troubleshooting section of
this manual (figure 3.2).
32397 Rev C1-2
3-1
Figure 3.2 – Referenced and ready to use
Using Tormach PCNC 1100 Series 3
Making your first part
Note: It is important to reference the PCNC before using it. Failure to do so can result in
running into the limit switches or, worse, the tool attempting to cut into the vise or table. The
Control Program tries to protect you from this sort of trouble but intentionally leaves the
responsibility of referencing to you. You can repeat the referencing operation at any time if you
have reason to suspect that the PCNC is in the wrong position (e.g., an error in a depth of cut
has stalled the machine).
Despite the advantages of having the machine referenced, you can still use it without, for
example if one of the home switches fails or becomes unreliable. We advise you to treat this as
a crippled mode for use until you can get the switch fixed. The Goto toolchange position macro
M998 will not work if the machine is not homed but you can ignore the error message and jog
the axes by hand to get clearance to change the tool.
The Control Software now knows exactly where the PCNC axes are and has called this home
position X = 0.0, Y = 0.0 and Z = 0.0. You probably think that this position is not very
convenient and you are correct. The Control Software will let you define any other place to be
0, 0, 0 when you are running a part-program but will always keep a record of the machine
position using home as machine zero. Normally the axis DROs will show your coordinates for
the position but you can see the Control Software machine coordinates by clicking the Machine
Coords button. A big flashing LED warns you that you are not looking at your version of the
coordinates.
3.2
Loading a Demonstration
Program
The system comes with a demonstration
program in the file
C:\PCNC3\GCode\FirstPart.nc
Run the Control Software and make sure
the screen LEDs by Reset button are not
flashing and that the axes are referenced.
Click the OpenG button. You will be
given a Windows open file dialog.
Navigate to the G-code folder and open
the file (figure 3.3).
Figure 3.3 – File opening
You will see the code of the program in
the window at the left of the screen and the path that the tool will take in the toolpath display.
Use the mouse to drag with the lefthand button in the toolpath display to
rotate the display. It behaves as if it is
drawn inside a clear ball and the mouse
turns the ball.
So that you understand what is going to
happen we should look at the way this
file was produced using a Computer
Aided Design/ Computer Aided
Manufacturing (CAD/CAM) program.
The PCNC will produce parts designed
in any available industry standard tools.
Tormach offers a number of powerful,
yet reasonably priced software tools,
some of which are used as examples in
this manual.
Figure 3.4 – The drawing for FirstPart
Using Tormach PCNC 1100 Series 3
3-2
32397 Rev C1-2
Making your first part
The original drawing is shown in figure 3.4. It consists of the characters “PCNC” and an
irregular quadrilateral.
Having drawn the outline of the
part, we defined the material from
which it will be cut, the size of tool
to cut the letters ( ¼") , the depth of
the letters, the size of tool to cut the
recess (½") and the depth of the
recess. The program automatically
creates the part-program (G- and
M-codes) to make the part and can
display a visualization of the
finished work (figure 3.5). We will
discuss the options which you have
for designing your own parts in the
next chapter.
You should now be able to relate
the toolpath display to the part
illustrated
Figure 3.5 – CAD/CAM Visualization of finished part
3.3
Running the Demonstration Part-program
3.3.1
Part Material
We suggest that you use a free-cutting
material to make this first part. MDF,
birch ply or, as we used, resin
impregnated ply are all suitable. You
need a piece at least ½" thick and 7" by
4". Clamp this securely to the PCNC
table. For many jobs it is worth putting
a layer of scrap material under the
work. This will protect the table when
through holes are to be cut and may
save damage in the event of a mistake
in the part program or in operating the
machine.
Figure 3.6 – Tool setup at zero points
Put a ¼" diameter tool into a tool
holder in the spindle. Ensure the lower
spindle pulleys are selected on the
machine and are set on the screen using
the Hi/Lo button.
Use masking tape to indicate a 5" length
near the middle. This length must be clear
of the clamps.
3.3.2
Setting Work Offsets
Jog the axes so that the tool is just above
the material at the top left-hand corner of
the 5" section (figure 3.6).
We suggest that you do a dummy run
cutting in the air so jog the Z-axis up
32397 Rev C1-2
Figure 3.7 – Toolpath during a cut
3-3
Using Tormach PCNC 1100 Series 3
Making your first part
about two inches.
Now click in the X-, Y- and Z-axis DROs, in turn and type
the value 0 into each of them. Do not forget to press Enter
to accept the values. The reason for doing this is that you
want the position of the tool (i.e., at the top left of your
material and an inch above it) to be X = 0, Y = 0 and Z =
0. The Control Software still refers to the home switches as
zero internally but lets you have your own separate
coordinate system for the work. If you click the Machine
Coords button then you will be shown how your zero
relates to the home position. The difference between the
machine coordinates and your coordinates is called the
Work Offset.
Figure 3.8 – Touching a tool
Note: We are going to cut this part by giving you a "recipe". You will learn why and how it
works later. Please don't add anything extra to the recipe. Adding yeast to a soda bread recipe
makes a fine mess. For example, here, you should have the length of each tool in the tool table
still set to zero.
You are now ready to run the program.
3.3.3
Cutting in Air
Click the Cycle Start button. The PCNC will start running but almost immediately ask for tool
number 1. This is already loaded so just click Cycle Start again. The machine will trace the
letters PCNC in the air. It does this four times because they are to be cut 0.2" deep and the
program is designed only to cut 0.05" each time. This is conservative but runs no risk of
breaking the ¼" diameter tool.
The toolpath shows the tool as it moves by a different colored line (figure 3.7).
After “cutting” the letters the machine will stop and ask for tool number 2. Jog the Z-axis up a
few inches so you can put the ½" cutter into the tool holder. Then jog down to about 2" above
the material, and type the value 0 into the Z DRO. Do not forget to press Enter to accept the
value.
Now click Cycle Start again. The machine will use a spiral path to cut out the recess (called a
pocket).
3.3.4
Cutting the Actual
Part
You should now be ready
to actually cut the part.
Jog the Z-axis and swap
back to the ¼" tool. You
must now set this so it is
just touching the surface
of your material and
define this as Z = 0. There
are many good ways of
doing this and we will
look at them in a later
chapter. For now you just
need a thin sheet of paper
or perhaps a plastic
wrapper from a candy
packet.
Using Tormach PCNC 1100 Series 3
Figure 3.9 – Cutting the text
3-4
32397 Rev C1-2
Making your first part
Jog the Z-axis down to ¼" or so above the material. If you are using keyboard jogging, change
the Slow Jog % DRO from 10% to 2%. The Tormach Jog/Shuttle Controller allows you to
control the speed depending on how far you turn the ring.
Then with the paper below the tool, carefully jog down until the paper just gets trapped by the
tool. You must avoid ramming the tool into the material; you want to just touch the paper
(figure 3.8).
When in position type 0 and Enter into the Z-axis DRO. You now have the Work Offsets set to
suit your material thickness and length of tool.
Make certain you have properly shut the door protecting the motor and spindle belts or the
spindle will not start and a non-rotating tool will try to cut the work.
Click Cycle Start. The program will stop for a tool change to tool 1. Just click Cycle Start as
you have tool 1 already
in the spindle.
The PCNC will cut the
letters in four passes.
Figure 3.9 shows this
process in pass two.
When the text is done the
machine will stop and
request a change to tool
2. Jog up so you can
change the tool to the ½"
cutter. If you hold the
Shift key down when
jogging the jog will take
place at full speed rather
than the 2% used for
very careful positioning.
Change the tool and jog
down with the paper
under the tool. Type 0
and Enter into the Zaxis DRO to define the
new Work Offsets.
Again check that the
door is shut.
Figure 3.10 – Cutting the pocket
Click Cycle Start to run
the program to cut the
pocket. Figure 3.10
shows this partially
done.
When the pocket is
completed the machine
will stop and rewind
the program so it can
be used to cut another
copy of the part.
Figure 3.11 – The completed part
The completed piece is
shown in Figure 3.11. You can compare this with the CAD/CAM visualization in figure 3.7.
32397 Rev C1-2
3-5
Using Tormach PCNC 1100 Series 3
Making your first part
3.3.5
Summary
This chapter has allowed you to make your first part with the PCNC. Although it is fairly
simple it would be very difficult to make without a CNC machine. When you are experienced
you should be able to design and make something like it from scratch in about 45 minutes.
You might have wondered about some of the things that you were told to do. Why did you cut
the text then remove half its depth with the pocket? Could the system be told how long each
tool is so you do not need to touch tools each time you make a part? Could the part be made in
steel with the same program?
These are all good questions. What you were told to do was to make this first part in the easiest
way not necessarily the quickest or most accurate. Subsequent chapters will tell you the
answers to these questions and give you the understanding to make the right design and
manufacturing decisions for yourself. This experience and understanding will be invaluable
whether you make production parts yourself or your designs are manufactured by others.
Using Tormach PCNC 1100 Series 3
3-6
32397 Rev C1-2
From an idea to a part
4.
Routes from an Idea to a Part
This chapter describes the different ways in which you can define parts to be
made with the PCNC.
It explains, in detail, how to use those features which are supplied built-in to or
bundled with the PCNC Control Software.
4.1
Controlling the PCNC
If you have run the sample program used in the previous chapter then you will have seen the
control language of the PCNC scrolling through the G-code window as it is executed. Although
this may look complex it is actually very simple. It was originally designed for machines whose
computer was comparable in power to the one in a microwave oven or multifunction TV remote
control!
Manual Keyboard
Controls
Keyboard
Direct Code
Entry on MDI
G0 X2.1 Y3.4
PCNC 1100 Software
G0
X2.1 Y3.4
G90G80G49
G0 Z20.0000
S1000
G0 Z20.0000
G0 X2.8521 Y3.0343
M3
f239.000 G1 Z0.0000
f239.000 G2 X2.5087 Y3.6823 I3.2919
G1 X2.5087 Y6.6988
G2 X2.8521 Y7.3468 I3.2919 J6.6988
G1 X3.8022 Y7.3468
G2 X4.1456 Y6.6988 I3.3623 J6.6988
G1 X4.1456 Y5.7764
G3 X4.4890 Y5.1284 I4.9288 J5.7764
G1 X5.5160 Y5.1284
G3 X5.8594 Y5.7764
Run Code Program File
M & G Code
Program File
Computer
hard disc
Standard Text Editor
(Microsoft Notepad)
PCNC 1100 Wizards
(Conversational Programming)
DXF, HPGL, JPG
File Conversions
CAD / CAM Program
Methods to Create Program Files
Figure 4.1 – Schematic on how to generate part-programs
The PCNC is always controlled by commands in a part-program. Most of these are G-codes
although many other letters are used to define the details like the spindle speed, feed rate, etc.
which are required. Thus a part-program is sometimes referred to as a G-code program.
Movement of the machine axes is controlled by three different G-codes.
32397 Rev C1-2
4-1
Using Tormach PCNC 1100 Series 3
From an Idea to a part
•
G00 moves at the maximum speed of the machine so is used when no cutting is required
•
G01 moves in a straight line between two points at the set feed rate
•
G02 (and G03) move in a circular arc between two points in a plane and possibly in a
straight line in other direction (e.g., to make a spiral).
All the moves take place from the current position of the tool. G00 and G01 need the
coordinates of the ending position (e.g., G01 X3.2 Y2.1 Z -0.3 would move the three
linear axes together so the tool will follow a straight line ending at X = 3.2, Y = 2.1 and Z = 0.3). G02 and G03, clockwise and counterclockwise arcs respectively, need additional
information to define the center point to be used.
Most G-codes are what is termed Modal. This means they stay in effect until another one is
used. So if G01 has been used on one line of code then the following lines only need to give the
position of the end of the move. As an example the following code will move the tool to a start
position (X = 1, Y = 2) and then move it in a square of side 3.1.
G00 X1.0 Y2.0
G01 X4.1
Y5.1
X1
Y2
In practice, however, the simplicity of G-codes is deceptive. Calculating the position of the
“center” of the tool by hand is tedious and error prone. If you wanted to cut around the outside
of a block of material to make the 3.1" square then you need to allow for the diameter of the
tool and need to move the Z-axis to take acceptable sized cuts in each of several passes.
You will easily be able to learn what a part-program is intended to do but it is unusual to write
one by hand as there is a wide range of software tools that can help you (figure 4.1).
4.2
Choosing the Appropriate Design Software
A mill is capable of producing three different classes of work which are usually referred to as
3D, 2½D and 2D.
A 3D product has complex and often smooth curves in all three dimensions. A typical example
is a mold for die-casting, vacuum forming or injection molding.
A 2½D product has detail at several depths from the surface of the material but each piece of
detail has a flat bottom surface. The FirstPart cut in Chapter 3 is an example of a simple 2½D
component.
A 2D product has no changes in depth. This might be a mechanism link cut out of a sheet of
steel or lettering cut out of vinyl sheet. 2D products can be milled but are usually produced on
specialist machines (e.g., a laser table or plasma cutter).
Design and particularly production of a 3D shape is much more time consuming than
something which is 2½D. If the pocket in FirstPart had a dished shape with a fillet in the
corners then it would have been cut with a ball nosed tool and would have required many
passes a few thou apart rather than the passes about 0.3" apart that could be used with the flat
end mill. In addition the design process is complicated because the pocket cannot be defined by
a single number (i.e., its depth) if it is 3D.
With current CAD software you will probably find it is easiest to design 2½D parts with a 2½D
CAD package or with a full 3D one running in 2½D mode.
4.3
Software for CAD/CAM
This section gives some guidance on things to consider when choosing software. It is a very big
topic whose surface we try to skim.
Using Tormach PCNC 1100 Series 3
4-2
32397 Rev C1-2
From an idea to a part
The two most important points are that (a) the PCNC, because of its open and standard
architecture, will run the part-programs produced by virtually all Computer Aided
Design/Computer Aided Manufacture (CAD/CAM) software and (b) that the more
comprehensive the software that you use, the greater will be your and the PCNC’s, productivity
and the better the quality of the parts made. A common mistake is to purchase inadequate
design software and then have to discard it and the investment made in learning to use it.
The Control Software itself includes features for defining and cutting simple parts like
keyways, rectangular and circular pockets or a plane face by conversational Wizards. You will
be able to do useful work with these features but you will get better control and documentation
of your parts be using a dedicated CAD/CAM system. Some software integrates the “drawing”
(CAD) and G-code production (CAM) functions but it is equally common to use different
programs from different suppliers for the two functions.
It is perfectly possible and often efficient to design using a 3D CAD package and machine with
a 2½D CAM package.
4.3.1
3D CAD
3D CAD software has the biggest range of purchase cost and the steepest learning curve. If you
want to produce true 3D parts like molds then you have no option but to buy the best package
you can afford. Alibre produces a good example of a mid-range 3D CAD package and Alibre
Design XPress is bundled with the PCNC 1100.
Alibre allows you to design parts by extruding 2D shapes. The extrusions can be from different
planes or surfaces of the part as it is built up and can be solid
material or holes.
Several parts can be put together into an assembly and conventional
orthographic engineering drawings more or less automatically
produced from the model.
High-end programs like Solidworks and Pro/ENGINEER also work
in the same way and can be used to design for manufacture with the
PCNC.
A 3D CAD program will typically allow the export of solid models
(IGES or STL format) for input to a 3D CAM program or DXF
format files for use in 2½D CAM.
4.3.2
Figure 4.2 – Keyhole
2D CAD
In a 2D CAD program you represent parts
by drawing the individual views of the
engineering drawings. A vast range of
software is available (much of it “free”).
We advise that you use software that allows
you to express the “intent” of your design
in the drawings rather than just drawing a
set of lines.
Figure 4.4 – Joined
As an example let us assume you want to
Figure 4.3 – Line moved
points
make a key-hole shaped slot in a block of
but line moved
material. This can easily be drawn as two
arcs and two lines with the hole that accepts the key’s shank being highlighted (figure 4.2).
How useful this drawing is depends of how intelligently the CAD program can interpret the
lines. As drawn they are probably separate and can be moved independently (figure 4.3). Most
software will allow joining the lines so they move together (figure 4.4). This however does not
really reflect what the part is like.
32397 Rev C1-2
4-3
Using Tormach PCNC 1100 Series 3
From an Idea to a part
The important things about the intent of this design are that the straight lines should be parallel
and the same length and that they form a tangent to the arc at the bottom of the slot. If these
constraints can be given to the CAD software then it will be possible to change its sizes (e.g.,
the width of the slot by dragging the radius of the bottom arc) while
retaining the shape (figure 4.5).
If the shape is defined like this then the software can display the
minimum set of dimensions required to define it (figure 4.6). Finally
if a dimension is changed then the part can be redrawn to
correspond to the new size (figure 4.7).
4.3.3
CAM
We have seen the sort of features you can get from a CAD program.
Figure 4.5 –
Constrained and
There are also big differences between different CAM programs.
size changed
Some CAM programs accept 2D models (drawings) of your part
(e.g., DXF) files and expect you to define the Z depth of features like pickets, engraved text and
holes. Alternatively a 3D CAM program will find all the dimensional information in the model
Figure 4.6 – Automatic dimensions displayed
Figure 4.7 – Changed dimension
changes drawing
(e.g., IGES) file.
The main issues to consider are how many times you need to tell the CAM program how to
machine the part and how good a visualization of the part you will be shown.
Suppose we decide that the inside of the keyhole slot is to be cut with a 0.125" end mill using
Figure 4.8 – Path of tool and G-code
Using Tormach PCNC 1100 Series 3
4-4
32397 Rev C1-2
From an idea to a part
conventional milling to a depth of 0.5" with each pass being 0.1" deep. The CAM software will
generate a G-code program for this.
In some freestanding CAM software, if the size of the slot is changed so the drawing changes,
then you would have to create the pocket G-code for the slot from scratch with each revision of
the drawing. Integrated CAD/CAM software will work dynamically with the CAD and
automatically recreate the new G-code with each change in dimension.
A reasonably sophisticated CAM program will give you a choice of views of the finished part
and the path of the tool as it is manufactured.
Figure 4.8 is a screen shot of a typical CAD/CAM program and shows the toolpath for one
version of the slot. It is shown in a plan view together with a pane which displays the G-code
generated to perform the operation.
Figure 4.9 is the result of retyping the radius of the end of the slot as 0.15" and displaying a
rendered isometric view of the part. The G-code (moved into a smaller pane for clarity on the
rendered view) was automatically updated to reflect the new slot width.
Figure 4.9 – Rendered Isometric view of narrower keyhole slot
32397 Rev C1-2
4-5
Using Tormach PCNC 1100 Series 3
From an Idea to a part
4.3.4
Running the G-code
Figure 4.10 – Keyhole loaded and ready to run
The CAM program will write the G-code part-program to disk. Assuming you are using a
different computer to design your part from that controlling the machine you need to transfer
the file to the hard drive of the control computer. Then you can load and run it in the same way
you did for the FirstPart program. Figure 4.10 shows the keyhole loaded into the Control
Software.
Note: Do not attempt to run part-programs off a USB key drive or floppy disc.
4.3.5
CAD/CAM Systems
Vectric Cut 2D is a 2½D system which will accept DXF drawings from virtually any source,
has powerful features and is very easy to learn. If you already have a favorite CAD program
then this will be a good choice for you to do CAM work.
Figure 4.12 – Model for mount
Figure 4.11 – Motor Mount DXF
Figure 4.11 shows a DXF drawing of a mounting plate for a motor. This was produced from the
solid model in figure 4.12 but could have been drawn with virtually any program.
Using Tormach PCNC 1100 Series 3
4-6
32397 Rev C1-2
From an idea to a part
Figure 4.13 – Cut2D job for Motor Mount
Figure 4.13 shows the drawing loaded as a Cut 2D job
If your work needs
powerful parametric
solid modeling and 3D
milling from these
models then the matched
combination of Alibre
Design and SprutCAM is
available from Tormach.
Figures 4.14 through
4.16 illustrate a part
being designed in Alibre,
the manufacture being
defined in SprutCAM
and a finished test piece.
Figure 4.14 – Modelling a 3D part
32397 Rev C1-2
4-7
Using Tormach PCNC 1100 Series 3
From an Idea to a part
Figure 4.15 – Defining the machining technology
Figure 4.16 – The machined test piece
Virtually any other commercially available CAD/CAM systems can be used with the PCNC
control software because of its compliance with industry standards. CAD/CAM software is
configured to generate appropriate code for a particular machine tool by a post-processor. You
should consult Tormach for advice on the best post-processor option to purchase with your
preferred software.
Using Tormach PCNC 1100 Series 3
4-8
32397 Rev C1-2
From an idea to a part
4.4
Programming with Wizards
There will be situations when a simple piece of one-off machining has to be performed and you
do not have suitable CAD/CAM software or, perhaps, the machine user is unfamiliar with the
software that is available. The
Wizard facility built into the
Control Software is an ideal
solution.
4.4.1
Machining Wizard Concept
A Wizard is a special screen that is
displayed on demand by the
Control Software. It has a series of
DROs with which you define the
cuts that need to be made. Figure
4.17 shows the general appearance
of a surfacing Wizard.
4.4.1.1
Figure 4.17 – General view of a typical Wizard screen
Selecting and Running a Wizard
The Wizards>Pick Wizard menu displays a list of Wizards which are installed on your control
computer. Wizards can be obtained from a variety of online sources and you can modify a
standard one or write your own from scratch. Figure 4.18 shows an example of what the list
could contain.
Click on the Wizard that you want to use and click Run. Notice that a list that is too large to fit
in the dialog has a scrollbar but, rather unusually, it is on the left hand side of the list. The
Wizard screen will replace the screen currently visible.
4.4.1.2
Standard Wizard Features
Figure 4.19 shows a Wizard
for milling a circular
pocket.
As many different authors
write Wizards, there are
detailed differences
between the screens but
each one should have the
following:
•
Save Settings
button. This causes
the Control Software
Figure 4.18 – Wizard selection list
to remember the
values in each DRO so they will be available next time you choose the particular
Wizard.
•
Post Code button. This causes the Wizard to generate a G-code program to cut the shape
with the sizes you have specified. Most Wizards have a toolpath window and you will
see the cuts to be made in it. You can manipulate the toolpath display in the usual way
with the mouse (Rotate, Zoom if Shift depressed and Pan if Right-button drag)
•
Exit button. This returns you to the screen that was displayed before you ran the Wizard
in preparation for running its code.
•
An error line and button to Clear the text from it. This will display any problems found
trying to post code using the values that you defined.
32397 Rev C1-2
4-9
Using Tormach PCNC 1100 Series 3
From an Idea to a part
Note: A common problem when filling in the DROs of a Wizard is to forget to press Enter to
accept each value. It is easy to type a value and click in the next DRO. This discards the typed
value.
Figure 4.19 – Circular Pocket Wizard
4.4.1.3
G-code from a Wizard
You should carefully check the code generated by a Wizard – particularly if it is one which you
have not used before.
Things to look out for are:
4.4.1.4
•
Whether the Wizard sets a speed for the spindle (S-word) and starts it and how it
controls the coolant;
•
If any motion will conflict with clamps for your work;
•
Which position on the work piece the Wizard considers to be X = 0, Y = 0. A good
check is to define Z = 0 to be a plane a few inches above your work piece and do a test
run of the Wizard’s code.
Commercial Wizards
While many Wizards are bundled free of charge with the PCNC, a set from New Fangled
Solutions is a trial version of a product which requires a separate license. You can use all its
features to evaluate what the Wizards can cut but, without the license, you cannot actually
produce the G-code part-program.
Using Tormach PCNC 1100 Series 3
4-10
32397 Rev C1-2
Machine controls
5.
Machine Controls
This chapter gives a description of all the PCNC controls on the operator’s panel
and the Control Program screens.
If you have been through the section “Running the PCNC” in Chapter 2 you
already have a good grounding and may wish to skim through this chapter on
first reading of the manual and come back to it when you want to understand
exactly how some feature works.
5.1
Machine Operation
5.1.1
Operator’s Panel
The operator’s panel is illustrated in figure 5.1. It generally controls the PCNC directly and is
independent of the software in the control computer. When the Spindle and Coolant
switches are in the Auto position then control of these functions is given to the computer.
Figure 5.1 – Operator’s Panel
Main Switch
The main switch is mounted on the right hand side of the control cabinet. A padlock can be
inserted to lock it in the off position. It controls the 230 volt power to the main machine and the
separate power from the IEC inlet under the control cabinet to the computer and coolant
system.
Note: Disconnect the machine from the wall outlets before opening the control cabinet door as
it is possible that live terminals can be touched even when the isolator is in the OFF position.
32397 Rev C1-2
5-1
Using Tormach PCNC 1100 Series 3
Machine Controls
Warning: The following power-up and power-down sequences should be followed exactly to
avoid the risk of unintended machine motion which could cause injury to you or damage to the
machine. The control computer should always be booted-up and the Control Software run
before the green start button applies power to the mill axes and spindle. Similarly power off the
mill before shutting down the Control Software and the computer.
Computer On/Off
This rocker switch controls the power from the IEC inlet to the two outlets that are intended for
the computer and monitor. This is provided for convenience. In some applications the
computer/monitor might be powered directly from a wall outlet and this “computer” circuit left
unused or used for other functions such as to powering a work-light.
Start and EStop
The Start button will energize the circuits for the axis drives and for the spindle motor. The
Stop button, which locks in once pressed, stops all motion and is the Emergency Stop (EStop)
control. The Stop button is released by a turning the button-head a quarter-turn clockwise.
Machine start is protected by a no-volt relay from failure of the mains supply. The PCNC
requires Start to be pressed on re-application of power.
Status LEDs
The Machine LED indicates that the Start button has been pressed. When it is lit then the
Machine OK LED on the computer screen should be solid green.
The Computer LED indicates that the Control Software is running.
Spindle
An important safety interlock is that the rotation of the spindle can be disabled (while
maintaining axis drive power) by the Spindle Lockout key-switch. The switch on the beltguard door performs the same function. These are used to ensure that the spindle cannot start
when an R8 tool holder is being changed (door open) or when a tool is being changed in a collet
chuck.
The controls above the key-switch are all concerned with manual control of the spindle. If the
Manual/Auto switch is in Auto position then none of the other panel spindle controls have
any effect. In the Manual position the computer cannot control the spindle.
The rotary control potentiometer (RPM x 100) controls the speed on the spindle when it is in
Manual mode. Its legend indicates approximate spindle speed in the two pulley ranges.
The Spindle Start spring loaded rocker starts the spindle and the Spindle Stop rocker
stops it. The direction is determined by the setting of the Forward/Reverse switch. Forward
corresponds to clockwise rotation of the spindle. You can safely switch direction while the
spindle is turning.
Coolant
The Coolant switch controls the power from the coolant pump outlet on the underside of the
control cabinet. In the Off position the pump does not run. In the On position it runs
irrespective of the computer control. In the Auto position it will run if the Control Program
requests coolant.
Accessory Socket
The Accessory socket is for connection of accessories such as a touch probe.
Using Tormach PCNC 1100 Series 3
5-2
32397 Rev C1-2
Machine controls
5.1.2
Tool Changing
5.1.2.1
Tooling Strategy
The PCNC uses a R8 spindle and so
you have access to a vast range of
standard tooling. The main options
open to you are:
•
Tormach Tooling System
(TTS) – this allows you to
have all the tools that you
commonly use mounted in
low cost tool holders and to
change them very quickly.
The working length of each
tool is accurately maintained
each time it is loaded into the
spindle so it can be used for
cutting with no further setup.
Tool lengths can be setup
and checked in a stores or
inspection area without using
the PCNC (figures 5.2 &
5.3).
Figure 5.2 – Holders in the TTS range with collet
•
R8 tool holders – offer similar features to TTS
holders but need to be setup once in the machine
and are slower to exchange (figure 5.4).
•
Screwed shank cutter collet chuck
(Clarkson/Posilok type) – allows you to
exchange a cutter while maintaining a known
length as the center hole at the back end of the
cutter registers in the chuck (figure 5.5).
•
ER or similar collet – accepts a wide range of
cutter diameters but the length of the tool is not
accurately repeatable so the offset needs to be
reset after each tool change (figure 5.6).
•
R8 collet – gives the shortest overhang from the
spindle nose but requires an individual collet for
each tool diameter and, as with ER collets,
length is not repeatable.
The tool changing procedure is slightly different
depending on the tool-holders you have.
5.1.2.2
Figure 5.3 – TTS presetting
Changing R8 Tools
Open the spindle drive cover.
Swing the spindle locking fork so it
engages with the flats on the upper part of
the spindle. You will have to turn the
spindle a little to get it to line-up.
Figure 5.4 – R8 tool-holder
The locked spindle is shown in figure 5.7
32397 Rev C1-2
5-3
Using Tormach PCNC 1100 Series 3
Machine Controls
To remove any installed tools:
•
Wipe any debris from the spindle nose and the
tool being removed to avoid any risk of it
getting into the spindle bore;
•
Using the supplied 13 mm wrench on the
squared end, loosen the drawbar by about one
turn. Tap the end of it with a copper-faced
hammer to disengage the R8 taper;
•
While holding the tooling in one hand, fully
unscrew the drawbar and remove the tooling.
To insert a new tool:
5.1.2.3
•
Check that the R8 taper on the toolholder/collet is quite
clean;
•
Insert the toolholder/collet into the
spindle turning it to
ensure that the drive
keyway engages with
the key in the spindle.
Start the drawbar
thread to retain the
tool-holder/collet;
Figure 5.5 – Autolock chuck
Figure 5.6 – ER32 collet tool holder
•
If you are using a tool-holder then the
drawbar can be tightened. Otherwise,
using the drawbar to prevent the collet
jaws from closing in the spindle taper,
insert the TTS holder or tool into the
collet. Then tighten the drawbar.
•
Finally disengage the locking forks and
close the door.
Changing TTS Tools
For more information on the Tormach
Tooling system, please review the TTS
manual from the Tormach web site titled
"31866_TTS_Manual.pdf". For detailed
reading on the subject, feel free to read up on
"Preventing Collet Slip" in the Engineering
Documents section of the web site.
The system uses a precision ¾" R8 collet in
the spindle. Insert this as described above for
R8 tooling.
Figure 5.7 – Spindle lock fork engaged
Tool holders can be changed by loosening the
drawbar by just one turn and using the copper-faced hammer on the squared end to disengage
the collet taper. You do not need to remove the collet.
Note: You can change the tools in TTS drill chucks or the ER collet adaptor while these are
fitted to the PCNC spindle although doing this will not exploit the pre-settable nature of the
tools. You should use both spanners on the ER chuck rather than relying on the holder not
turning in the ¾" collet.
Using Tormach PCNC 1100 Series 3
5-4
32397 Rev C1-2
Machine controls
If you change a cutter or drill without opening
the door to lock the spindle you should use the
Spindle Lockout key to avoid any risk of the
spindle starting. If the door is open the spindle is
automatically inhibited.
Note: the draw bar is a wear part. After many
repeated tool changes, the draw bar will become
worn both at its threads, and on the shoulder near
the top. This wear can adversely affect your
ability to tighten tools properly. Inspect your
draw bar regularly and replace as required.
5.1.3
Spindle Speed Ranges
The PCNC has two speed ranges. The low range,
100 to 2000 RPM, is suitable for most machining
operations with ferrous and other tough
materials. The high range, 250 to 5140 RPM is
suitable for small diameter cutters and plastics
and non-ferrous materials.
Figure 5.8 – Changing spindle speed range
The range change is performed by moving the V-belt from the motor from the top pair of
pulleys (high speed range) to the lower pair (low speed range).
To change the belt position:
•
Open the protective door. Use the rear handle to unlock the motor mounting plate and
pull the motor forwards. The belt will slacken and can be moved from one pulley to
another (figure 5.8). It is slightly fiddly to get the belt through the slot between the
bottom pulley and the head casting.
•
Retighten the belt so there is between 1/8" and ¼" belt movement midway between the
pulleys. Lock the motor mounting and stow the handles in the vertical position.
5.2
Screen Control Panels
5.2.1
Using the Screens
Although at first sight you may feel daunted by the range of options and data displayed by
Control Software, this is actually organized into a few logical groups. We refer to these as
Families of Controls. By way of explanation of the term “control,” this covers both buttons and
their associated keyboard shortcuts used to operate the software and the information displayed
by DROs (digital read-outs), labels or LEDs (light emitting diodes).
The elements of each control family are defined for reference in this chapter. The families are
explained in order of importance for most users.
You should, however, note that all the screens of your system do not include all the controls
of a family. This may be to increase readability of a particular screen or to avoid accidental
changes to the part being machined in a production environment
5.2.2
Families of Related Controls
5.2.2.1
Screen Switching Controls
32397 Rev C1-2
5-5
Using Tormach PCNC 1100 Series 3
Machine Controls
These controls appear on each screen. They allow switching between screens and also display
information about the current state of the system (figure 5.9).
Reset
Figure 5.9 – Screen switching control family
This is a toggle. When the system is Reset the LED glows steadily.
Error and Profile Information
The Machine OK LED indicates that the PCNC is started.
The “intelligent labels” display the last “error” message, the current modes, the file name of the
currently loaded part-program (if any) and the Profile that is in use.
The Clear button clears the text from the error line. The entries written to the error line are
logged in the file C:\PCNC3\LastErrors.txt. This can be opened and inspected with a text
editor like Notepad if you want to analyze a history of events.
Screen Selection Buttons
These buttons switch the display from screen to screen. You are viewing the screen whose label
is blue. The keyboard shortcuts are given after the names. For clarity they are letters are shown
in upper-case. You should not, however, use the shift key when pressing the shortcut.
5.2.2.2
Axis Control Family
This family is concerned with the current position of the tool, or more precisely, the controlled
point (figure 5.10).
The axes have the following controls:
Coordinate Value DROs
These are displayed in the current units (inch/metric = G20/G21). The value is the coordinate of
the controlled point in the displayed coordinate system. This will generally be the coordinate
system of the current Work Offset (initially 1 – i.e., G54) together with any Tool length offset
and G52/G92 offsets applied.
If the X and Y coordinates display in red then they have been rotated by a G68 command.
You can type a new value into an Axis DRO. This will modify the current Work Offset to make
the controlled point in the current coordinate system be the value you have set. You are advised
to set-up Work Offsets using the Offsets screen until you are fully familiar with working with
multiple coordinate systems.
Referenced
The LED is green if the axis has been referenced (i.e., is in a known actual position).
Many users prefer to always run the PCNC in the referenced state.
Using Tormach PCNC 1100 Series 3
5-6
32397 Rev C1-2
Machine controls
Each axis can be referenced using its Ref button or the linear axes can be referenced together
using the Ref XYZ button.
The De-Ref All button does not move the axes but stops them being in the referenced state.
Figure 5.10 – Axis control family
Scale
Scale factors for any axes can be set by G51 and can be cleared by G50. If a scale factor (other
than 1.0) is set then it is applied to coordinates when they appear in G-code (e.g., as X words, Y
words etc.) . The Scale LED will flash as a reminder that a scale is set for an axis. The value
defined by G51 will appear and can be set, in the Scale DRO. Negative values mirror the
coordinates about the relevant axis.
The G50 button executes a G50 command to set all scales to 1.0
Correction Radius
Rotary axes can have the approximate size of the work piece defined using the Rotational
Diameter control family. This size is used when making blended feed rate calculations for
coordinated motion including the 4th Axis. The LED indicates that a non-zero value is defined.
Jog/Shuttle Axis
The axis that is selected for jogging by the Tormach Jog/Shuttle Controller is indicated by a
LED by the top left corner of the corresponding DRO.
5.2.2.3
Jogging Control Family
Jogging can be performed in two ways: (a) using the keyboard (or optional Keypad pendant) or
(b) Using the optional Tormach Jog/Shuttle Controller
Keyboard Jogging
32397 Rev C1-2
5-7
Using Tormach PCNC 1100 Series 3
Machine Controls
Whenever the Jog ON/OFF button is displayed on the current screen then the axes of the
machine can be jogged using the jog hotkeys on main keyboard or a pendant keyboard
If the Jog ON/OFF button is not displayed or it is toggled to OFF then keyboard jogging is not
allowed for safety reasons.
There are two modes, Continuous and Step which are selected by the Jog Mode button and
indicated by the LEDs.
Continuous mode moves the axis or axes at the defined slow jog rate while the hotkeys are
pressed.
The continuous jog speed is defined as shown below but this can be overridden by pressing
Shift with the hotkey(s). A LED beside the Cont. LED indicates this full speed jogging is
selected.
The jogging speed used with hotkeys in Continuous mode is set as a percentage of the rapid
traverse rate for the axis and for the Windows compatible joystick as a percentage of the feed
for the given stick deflection by the Slow Jog Percentage DRO. This can be set (in the range
0.1% to 100%) by typing into the DRO. It can be nudged in 5% increments by the buttons or
their hotkeys.
Step mode moves the axis by one increment (as defined by the Step DRO) for each key press.
The current feed rate (as defined by the F word) is used for these moves. The size of increment
can be set by typing it into the Step DRO or values can be set in this DRO by cycling through a
set of predefined values using the Jog Step button.
Incremental mode is selected by the toggle button or, if in Continuous Mode temporarily
selected by holding down Ctrl before performing the jog.
Tormach Jog/Shuttle Controller
This jogging device is available as an
optional accessory (part number 30616,
figure 5.12).
Many users will find that it increases
their productivity, especially on shortrun jobs requiring a lot of setting up of
workpiece and tooling.
The four buttons starting at the left are
allocated to select jogging of axes X, Y,
Z and A respectively. A LED beside an
axis DRO indicates that this axis is the
one that will be jogged.
The fifth button cycle through the
available jog step sizes. Alternatively
you can type a step size into the Step
Figure 5.11 – Jogging control
family
DRO.
Figure 5.12 – Tormach Jog/Shuttle Controller
Continuous jogging is performed by
turning the spring loaded ring
counterclockwise for the minus direction and clockwise for the plus direction. There are seven
speeds, in geometric ratio, from very slow to full speed so you can position any axis with great
speed and precision.
The inner wheel (with finger dimple) will jog by one Step as defined in the Step DRO for each
click. The move will be made at the current feed rate.
Using Tormach PCNC 1100 Series 3
5-8
32397 Rev C1-2
Machine controls
5.2.2.4
Spindle Speed Control Family
The machine spindle can be controlled in two ways:
(a) by hand or (b) by switching to Auto on Operator’s
panel, thus making the speed and direction set by the
Control Software.
This control family is only important for case (b).
The S DRO has its value set when an S word is used
in a part-program. It is the desired spindle speed. It
can also be set by typing into the DRO (figure 5.13).
It is an error to try to set it (in either way) to a speed
greater than that displayed in Max Speed for the
chosen pulley and the nearest legal value will be
chosen.
The Hi/Lo button toggles between the two belt/pulley
settings with the LEDs indicating the configuration
(spindle on left, motor on right)
Figure 5.13 – Spindle speed
control family
The maximum available speed is indicated.
The S- and S+ buttons increase and decrease the value in the S DRO geometrically using a ratio
of 1.15 for each click on the button. This reflects the usual arrangement of gearbox in a manual
machine tool.
The spindle can be started in a clockwise direction by the Spindle CW button. An M-code (M4)
in the MDI box is required if you want to select counterclockwise running.
The main LED above the Spindle CW button indicates that the spindle is “running” – although
actual movement may be inhibited by the key and/or door interlocks. The two LEDs that flank
it indicate a Dwell while the spindle gets up to speed or fully stops.
The Coolant button and its associated LED control the coolant power outlet under the control
cabinet.
5.2.2.5
Feed Control Family
Feed Units per Minute
The F DRO gives the feed rate in current units
(inches/millimeters per minute). It is set by the F
word in a part-program or by typing into the F
DRO. The control software will aim to use this
speed as the actual rate of the coordinated
movement of the tool through the material. If this
rate is not possible because of the maximum
permitted speed of any axis then the actual feed rate
will be the highest achievable (figure 5.14).
Feed Units per Revolution
As modern cutters are often specified by the
permitted cut per “tip” it may be convenient to
Figure 5.14 – Feed control family
specify the feed per revolution (i.e., feed per tip x
number of tips on tool). In this case the F DRO gives the feed rate in current units
(inches/millimeters) per rev of the spindle. It is set by the F word in a part-program or by typing
into the DRO.
32397 Rev C1-2
5-9
Using Tormach PCNC 1100 Series 3
Machine Controls
Notice that the numeric values in the control will be very different unless spindle speed is
near to 1 rpm! So using a feed per minute figure with feed per rev mode will probably
produce a disastrous crash!
Feed Display
The actual feed in operation allowing for the coordinated motion of all axes is displayed in
Units/min and Units/rev . If the spindle speed is not set and the actual spindle speed is not
measured then the Feed per rev value will be meaningless.
Feed Override
Unless M49 (disable feed rate override) is in use, the feed rate can manually be overridden in
the range of 20% to 100% by entering a percentage in the (feed rate override) DRO with a %
sign. While it is possible to enter numbers higher than 100%, the practice is not recommended.
The LED warns if an override is in operation.
The control software will apply any changes in feed rate override as quickly as possible. This
could be very important if you decide you have too high a feed rate for safety. To optimize
performance, the software keeps a queue of moves ready to be implemented. It is possible if
you increase the federate that you will make one of these queued moves be faster than the
PCNC can move or accelerate and so it will loose steps. The best strategy is to write the part
program to run at the highest anticipated feed rate and then use the override at less than 100%
to reduce it to produce the best operating condition.
The FRO DRO displays the calculated result of applying the percentage override to the set feed
rate.
5.2.2.6
Program Running Control Family
These controls handle
the execution of a
loaded part-program or
the commands on an
MDI line (figure 5.15).
Cycle Start
Safety warning: Note
that the Cycle Start
button will, in general,
start the spindle and
axis movement.
Figure 5.15 – Program running family
Stop
Stop halts axis motion as quickly as possible. Unless used when Paused, it may result in lost
steps (especially on stepper motor driven axes) and restarting may not be valid.
Rewind
Rewinds the currently loaded part-program.
Single BLK
Single BLK is a toggle (with indicator LED). In Single Block mode a Cycle Start will execute
the next single line of the part-program.
Using Tormach PCNC 1100 Series 3
5-10
32397 Rev C1-2
Machine controls
Pause
Pause brings the current move to a controlled stop applying deceleration etc. Although jogging
while paused is possible we do not recommend doing it. The best sequence is to Pause and then
press Stop. Resume by editing the program or using the Run From Here feature.
Line Number
Line DRO is the ordinal number of the current line in the G-code display window (starting from
0). Note that this is not related to the “N word” line number.
You can type into this DRO to set the current line.
Run from Here
Run from here performs a dummy run of the part-program to establish what the modal state
(G20/G21, G90/G91, etc.) should be and then prompts for a move to put the controlled point in
the correct position to for the start of the line in Line Number. You should not attempt to Run
from here in the middle of a subroutine.
Set next line
Like Run from here but without the preparatory mode setting up processing.
Block Delete
The Ignore "/" Blocks button toggles the Block Delete “switch.” If enabled then lines of G-code
which start with a slash (i.e., / - will not be executed).
Optional Stop
The M01 Break button toggles the Optional Stop
“switch.” If enabled then the M01 command will
be treated as M00.
Goto Toolchange
This button provides manual movement of the
controlled point when the part-program is
stopped.
Tool Details
Controls display the current tool, its name, the
offsets for its length and diameter and whether the
offsets are active (ON).
Unless tool change requests are being ignored, on
encountering an M6 the Control Software will
stop and flash the Change Req LED. You
continue (after changing the tool) by clicking
Cycle Start.
Work Offset Details
The name of the current work offset coordinate
system is displayed.
5.2.2.7
Figure 5.16 – Toolpath and G-code display
family
Toolpath Control Family
The currently loaded part-program is displayed in
32397 Rev C1-2
5-11
Using Tormach PCNC 1100 Series 3
Machine Controls
the G-code window. The current line is highlighted and can be moved using the scroll bar on
the window (figure 5.16).
The Toolpath display shows the path that the controlled point will follow in the X, Y and Z
planes. When a part-program is executing, the path is over painted in green. This over painting
is dynamic and is not preserved when you change screens or indeed alter views of the toolpath.
On occasions you will find that the display does not exactly follow the planned path. This
occurs because the Control Software prioritizes the tasks it is doing. Sending accurate step
pulses to the machine tool is the first priority. Drawing the toolpath is a lower priority. It will
draw points on the toolpath display whenever it has spare time and it joins these points by
straight lines. So, if time is short, only a few points will be drawn and circles will tend to appear
as polygons where the straight sides are very noticeable. This is nothing to worry about.
The Simulate Program Run button will execute the G-code, but without any tool movement and
allow the time to make the part to be estimated.
The Absolute Motion Extremes data allow you to check if the maximum excursion of the
controlled point is reasonable (e.g., not milling the top of the table).
The toolpath display can be rotated by left clicking and dragging the mouse in it. It can be
zoomed by shift-left clicking and dragging and can be panned by dragging a right click.
The Regenerate button will regenerate the toolpath display from the G-code with the currently
enabled fixture and G92 offsets.
The Display Mode button will chose whether the default toolpath display is sized for the
machine envelope (as defined by the “soft limits”) or the object defined by the extremis of the
part-program.
The Jog Follow button allows the toolpath display to be automatically scrolled as the controlled
point is jogged.
5.2.2.8
File Control Family
These controls are involved with the file of your part-program. Most should be self-evident in
operation.
Figure 5.17 – File control family
Change G-code allows you to use the Notepad editor to edit the part-program you have loaded.
When clicked it displays the current file (figure 5.18).
5.2.2.9
Work Offset and Tool Table
Control Family
This family is explained in detail in
Chapter 6 (figure 5.19).
5.2.2.10 MDI and Teach Control Family
G-code lines (blocks) can be
entered, for immediate execution,
into the MDI (Manual Data Input)
line. This is selected by clicking in
it or the MDI hotkey (Enter). When
the MDI line is active its color
changes and a fly-out box showing
the recently entered commands is
Using Tormach PCNC 1100 Series 3
Figure 5.18 – Notepad to edit G-code
5-12
32397 Rev C1-2
Machine controls
displayed (figure 5.20). The cursor up and down arrow keys can be used to select from the flyout so that you can reuse a line that you have already entered. The Enter key causes the current
MDI line to be executed and the MDI remains active for input of another set of commands. The
Esc key clears the line and deselects it. You need to remember
that when it is selected all
keyboard is written in the MDI
line rather than controlling the
machine. In particular, jogging
keys will not be recognized – you
must Esc after entering MDI.
The Control Software can
remember all the MDI lines as it
executes them and store them in a
Figure 5.20 – MDI and Teach control family
file by using the Teach facility.
Click Start Teach, enter the
required commands and then click Stop Teach. The LED blinks to remind you that you are in
Teach Mode. The commands are written in the file with the conventional name
C:/PCNC3/GCode/MDITeach.tap. Clicking Load/Edit will load this file so it can be run
or edited in the usual way – you need to go to the Simple Run or Comp Run screen to see it. If
you wish to keep a given set of taught commands then you should Edit the file and use Save As
in the editor to give it your own name and put it in a convenient folder.
5.2.2.11 Loop Control Family
The Control Software can execute a partprogram many times, automatically
updating a limit to the depth to which the
Z-axis can move (figure 5.21).
The part-program must end with an M30
(rewind) code.
Figure 5.21 – Loop control
The number of passes you require is
entered into the Cycles DRO. The initial lowest Z position is put into Z inhibit (note this will
often be negative) and the distance Z is to move down each cycle is put into Z Step (usually
positive). The On/Off button enables the feature.
The Multipass button will prompt for the values by a series of dialogs rather than requiring the
DROs to be filled in.
5.2.2.12 Modes and Mode Alarm Control Family
Figure 5.22 – Current modes display
These families display the current modes
of the Control Software and an “alarm”
LED for unusual modes. The alarm is on
the Diagnostics screen. Click on the
flashing LED to see a list of unusual
modes (figure 5.22).
These modes might arise from running a
part-program produced by a CAD/CAM
system not customized for all the features
32397 Rev C1-2
5-13
Figure 5.23 – Unusual modes display
on Diagnostics
Using Tormach PCNC 1100 Series 3
Machine Controls
of the PCNC.
An unusual mode does not imply a fault in your system, simply a hint of what to look for if
unusual things are happening (figure 5.23).
If for any reason the standard modes do not suit your normal working then by double-click on
the unusual modes LED you can define the current state as “usual.”
5.2.2.13 Rotational Diameter Control Family
As described in the Feed Rate control family, it is
possible to define the approximate size of a
rotated work piece so the rotational axis speed can
be correctly included in the blended feed rate. The
relevant diameters are entered in the DRO on this
family (figure 5.24).
The Axis control Family has a warning LED to
indicate the setting of a non-zero value here.
Figure 5.24- Rotational diameters
Note: A value is not required if rotary movement is not to be coordinated with linear axes. In
this case a suitable F word for degrees per minute or degrees per rev should be programmed.
5.2.2.14 Toolchange Position Control Family
This family defines the place the machine should go to when a request to change a tool occurs
or when the Goto Toolchange button is clicked. A part-program can go to it by using the M998
code (figure 5.25).
The position is defined in
machine coordinates (i.e.,
relative to the home
switches) and in the default
machine units.
Enter the special value
9999 if you do not want a
given axis to move when a
tool change is requested.
The units in which you
define your toolchange
position can be configured
by the Toggle T/C Units
button.
Figure 5.25 – Tool change position
Note: The move will take place
correctly whatever units the machine is
in at the time and, because machine
coordinates are used, to a fixed place
irrespective of the offsets in use.
The tool change position is also used
when you want to use the central
lubrication system.
Figure 5.26 – Inhibits and overrides family
This family also allows you to set the machine coordinates used if your part-program executes a
G28. We advise you to use the M998 toolchange location whenever possible as this checks that
the machine is referenced (i.e., the machine coordinates are valid). G28 will use whatever
values are in use irrespective of them being valid because the machine is referenced.
Using Tormach PCNC 1100 Series 3
5-14
32397 Rev C1-2
Machine controls
5.2.2.15 Inhibits and Overrides Control Family
In testing a part-program it is sometimes useful to be able to inhibit the movement of an axis
(e.g., typically Z). This is done with the Axis Inhibit buttons (figure 5.26).
When an axis hits a limit switch it will trigger a software EStop condition so all movement
will cease. If Auto LimitOverRide is enabled then you can reset the system and carefully jog off
the limit. If you want more security in this situation you can disable AutoLimitOverRide and
click the OverRide Limits button before clicking Reset on each occasion.
5.2.2.16 Feeds and Speeds Calculator
Different materials and tooling require different cutting speeds and feed so you will need to use
published tables and your experience to define the optimum spindle speed and the feed rate for
any given job. A simple calculator on
the Settings screen will, however, do
the math for you when you know a
cutting speed (in feet per minute) and
a chip per tooth loading (figure 5.27).
Enter your cutting data into the
DROs, not forgetting to press Enter
for each value and click the Calc
RPM/Feed button. The screen labels
show the calculation that is being
done for you.
Figure 5.27 – Speed/Feed calculator
5.2.2.17 Tapping Configuration Family
The control software allows use of the Tormach Tapping Heads (PN 30612 and 30613) without
a detailed understanding of the sequence of moves that are needed to control the head. The
holes are tapped by using
one of the M-code macros
M871, M872, M873 or
M874. The macros work as
a kind on canned cycle.
Each macro is set up for a
particular pitch of thread
and choice of tapping head.
This information is
Figure 5.28 – Tapping Configuration
provided by the Tapping
Configuration family of
controls (figure 5.28).
The TPI or Pitch DRO is interpreted in a different way depending on whether the part program
calling its macro is running in Inch (G20) or metric (G21) mode. In G20 mode the value is a
number of threads per inch and in G21 mode it is the pitch of the thread in millimeters. It is
perfectly possible to change modes within a program and so have a job with mixed thread
standards. Fortunately Inch numbers are unlikely to be pitches and vice-versa. The control
software checks that the chosen pitch can be cut at the current spindle speed when the macro is
called so there is little chance of damage to a tap.
If you select Dwell mode then the macro will use an alternative movement algorithm which
dwells (pauses) at the bottom of the thread. This gives a more accurate depth but slower tapping
and more wear on the mechanism of the tapping head.
Both tapping heads have a high-speed reverse feature to minimize tapping time. As the gear
ratios are different for each head you must define which is going to be used by toggling to the
appropriate large or small LED.
32397 Rev C1-2
5-15
Using Tormach PCNC 1100 Series 3
Machine Controls
5.2.2.18 Misc. Settings Control Family
Current Units
This displays the units currently
selected (figure 5.29).
Ignore Tool Change
Normally when the part-program
calls for a different tool
execution will stop, the Tool
Change LED will flash and you
need to press Cycle Start to
Figure 5.29 – Misc. settings
continue. Tool change requests
can be ignored by clicking the
Ignore M6 Tool Change button. This can be useful when air-cutting to prove/time a part
program.
G73 Pullback
This DRO defines the distance that a high speed peck drill cycle (G73) will pullback when
breaking the chip. You may need to alter this value for metric use.
IJ Mode
The IJ mode defines how the I, J and K words in a G02 or G03 are interpreted. There is no
standard for this so different CAM post processors will use different conventions. The PCNC
usually runs with I, J and K being incremental distances from the current point. You can make
the Control Software treat them as absolute positions by clicking the Set Abs I/J button. The
symptoms of an incorrect setting are that small arcs can display a massive circle on the toolpath
or you get an error message about the radius of an arc being different at the start and end of a
cut.
5.3
USB Jogging Pendants
Optional accessories purchased by many users are the
USB jogging pendants. These provide access to the
main axis jogging controls on a unit that can be
positioned for use while touching-off the tool position.
They are not resistant to coolant and, for safety reasons,
do not have controls for starting and stopping
machining.
The pendants should be plugged into USB ports on the
computer motherboard. We have found connections
through hubs can lower responsiveness.
5.3.1
Figure 5.30 – Jog Wheel pendant
Jog/Shuttle Controller
The Jog /Shuttle Controller is a low cost but very precise and fast way of jogging the four axes.
There are five buttons and two rotary controls (figure
5.30).
The buttons allow you to select which axis you wish to
jog. The chosen axis is indicated by a LED next to the
corresponding DRO. For example, figure 5.31 shows that
the X-axis is the one to be jogged. If a Jog/Shuttle
Controller is not installed then all the LEDs will be dark.
The Step button will cycle through a set of jog step sizes
in the Step DRO in the Jogging family. The available
Using Tormach PCNC 1100 Series 3
5-16
Figure 5.31 – X-axis will be jogged
32397 Rev C1-2
Machine controls
preset step sizes can be customized with PCNC Config (see chapter 9)
The outer rotary shuttle control is spring-loaded. Turning it will jog the selected axis at a speed
proportional to the amount it is turned. There are seven different speeds arranged geometrically
so you have instant control from the full rapid speed (65 rpm) down to the slowest crawl.
The inner rotary control, operated by fingertip, has detents. Each click will jog at the current
feed rate by the distance defined in the Step DRO. If you turn it faster than the axis can move
the impossible steps will be ignored so the axis will never buffer up a backlog.
5.3.2
Keypad Pendant
The keypad pendant has two modes of operation. The
CNC/Num key toggles between these modes (figure 5.32).
When the Numeric LED is lit it is a conventional numeric
pad. It can be used for entering values into DROs. Note that
as Backspace in not available on the main keyboard during
DRO entry it cannot be used on the pendant either.
When the LED is not lit the majority of the keys are
concerned with jogging the four labeled axes (X, Y, Z and
A – keys 2, 3, 4, 6, +, 8, 9, - )
The 7-key will perform a Home All operation (homing Z to
limit switches and then X and Y).
The 1-key will toggle the state on the Optional Stop LED.
When the LED is lit, M01 is treated exactly like M00 (i.e.,
end program), otherwise M01 is ignored.
Figure 5.32 – Keypad pendant
The /-key toggles between Continuous and Incremental (or Step) jogging modes. In step, one
key press produces a single step axis movement. The step size is displayed in a DRO.
The *-key (labeled Size) cycles through the available Increment (Step) sizes.
32397 Rev C1-2
5-17
Using Tormach PCNC 1100 Series 3
Offsets
6.
Using Multiple Tools
This chapter explains how you can configure the PCNC to use several tools
without having to waste time at each tool change defining the length of the new
tool. It also covers techniques for simplifying machining of work in a vise or
other fixture.
Offsets used are often considered as advanced features but the design of the
PCNC Control Software should make them easy to use. You will find it
worthwhile to master this chapter even if it needs more than one reading to do
so.
6.1
Offsets and Coordinate Systems
If you made the FirstPart then you will already have met and used the ideas explained in this
section.
When you Reference the PCNC, when it is started, the X-, Y- and Z-axes are moved so that
they are just off the home switches and the machine coordinates are set to 0.0. We saw that this
is not useful when you want to run a part-program as the program will have its own view of
where zero should be; in the case of FirstPart this is the top left corner of the material for X = 0,
Y = 0 and the top surface for Z = 0. By moving the tool to this position and zeroing the axis
DROs you defined relationship between the Machine Coordinates and the coordinates which
the part-program would use – the Program Coordinates. The general term for the relationship is
Offsets.
6.2
Tool Length Offsets and the Tool Table
For a given machining operation the X and Y position of the workpiece will be fixed. However
you will often need to use several tools and as these will be different lengths then you need to
change the Z offset. The control software allows you to switch tools quickly and without the
need to set up the machine every time a tool is mounted. Each tool and holder only needs to be
“measured” once, either offline or in the machine.
If you do not have enough holders for all the tools for a job then you will need to set the Z
work-offset each time you load a new tool. Using the tool table is only useful if you can put
each tool into the spindle in a fixed position. Skip this section if you do not want to use the tool
table.
The following example demonstrates a typical sequence using the Tormach Tooling System
and setting up a “touch off” tool and 3
cutting tools in the tool table.
6.2.1
Example Operation of Multiple
Tools
The following example has three simple
steps
1. Fill the tool table with the tools
you plan to use
2. Zero to the work height
3. Apply the tool offset
32397 Rev C1-2
Figure 6.1 – The example set of tools
6-1
Using Tormach PCNC 1100 Series 3
Offsets
6.2.1.1
To fill the table:
Figure 6.2 – Open tool table
Figure 6.3 – Tool table
•
Select the three tools to use, we'll use the touch off tool as #1 and the cutting tools of drill,
end mill, and face mill as #2, #3 and #4
•
Use the Config menu to open the tool table (figure 6.2) . It will look something like figure
6.3
•
Using the TTS height gauge and the granite block, measure the tools, adding each one’s
name and length to the table. The touch tool (#1) length is measured when the dial reads 0.
Figure 6.4d
Figure 6.4a
Figure 6.4c
Figure 6.4b
•
Here are the measurements we took:
Tool Number
Description
Height
Tool #1
Tool #2
Tool #3
Tool #4
Touch Tool
Drill 3/16"
End Mill 3/8" rougher
Face Mill 1.5" face
7.084"
7.151"
4.396"
4.115"
The completed table will look like figure 6.5.
Note: The Diameter Wear and Height Wear values in the table should not have data in them as
they are ignored by the current version of the control software.
Using Tormach PCNC 1100 Series 3
6-2
32397 Rev C1-2
Offsets
Figure 6.5 – Data in tool table
Note: The values in this table are always in inches. If you want to input tool lengths in
millimetres then you can do this when you are in metric
(G21) mode by using the tool length part of the Offsets
screen.
If you change a tool, for example by sharpening it, if it
comes loose in its holder or fitting a new cutter, then
you must make sure you re-measure it on the granite
block and update the tool table.
6.2.1.2
Zeroing to work height
Here you are going to set the work offset of Z so tool
#1 is touching the top of the work when Z = 0.0. As the
tool table gives the lengths of all tools that means Z
will be zero when each tool in on the spindle and
selected from the tool table by its number.
•
Mount the touch tool (#1) in the spindle
•
Set the current tool by typing 1 (followed by Enter) into the DRO labelled T
•
Jog the Z axis down so the dial indicator touches the top of the work and reads 0.0 (i.e. the
Figure 6.6 – Selecting tool #1
Figure 6.8 – Setting work offset so Z = 0.0
Figure 6.7 – Dial zero touching work
32397 Rev C1-2
6-3
Using Tormach PCNC 1100 Series 3
Offsets
position of the pointer when you measured the tool length – remember the tool is upside
down now relative to when you measured it) (figure 6.7)
•
6.2.1.3
Click the Zero button on the Z Axis DRO (to set the work offset) (figure 6.8)
Using tool #2
•
Set the value 2 in the T DRO.
•
Mount tool #2 in the spindle.
The Z axis DRO now reads the distance between the tool tip and the work.
6.2.1.4
Using other tools
Repeat the above for any tool number that you have defined in the tool table
6.2.1.5
Changing to a different work-piece
All you have to do is repeat the Zeroing to work height process with the touch off tool when
you have clamped another work-piece in the vise or on the table.
6.2.2
How this multiple tooling setup works
As explained above the machine works with two types of coordinates:
Machine coordinates are really an internal function of the machine. It's the machine's way of
Figure 6.9 – A possible way of measuring coordinates
Using Tormach PCNC 1100 Series 3
6-4
32397 Rev C1-2
Offsets
keeping track the positions of its parts, like the height of the spindle head.
Program coordinates are what we worry about. Program coordinates are what shows up in the
normal axis DROs and they are the positions that most G code commands reference.
The conversion between program coordinates and machine coordinates is done by the offsets.
They apply to all linear axes, X, Y, Z and the rotary axis A. The way offsets work in Z is shown
in figure 6.9.
In the image above, it should be clear that the following equation applies:
Program Coordinates + Work Offset + Tool Length = Machine Coordinates
The tool length comes from the tool table. The work offset comes from the work offsets table,
also sometimes called the fixture table. There 255 different work offsets available. The first few
are called by G54 through G59. You can do virtually all straightforward machining using just
the one default work offset system (G54). You only need multiple systems if you decide to use
more than one vise or other complex fixturing clamps. We will talk more about the work offsets
later.
When we used the Z axis Zero button with the tool touching the top of the work, what happened
is that current value of the Program Coordinate was added to the current work offset. For
example, if we had the following before pressing the Zero button.
Machine Coordinate
Program Coordinate + Work Offset + Tool offset =
3
+
2
+
4
=
9
Then after the Zero button was pressed we would have the following result:
Machine Coordinate
Program Coordinate + Work Offset + Tool offset =
0
+
5
+
4
=
9
so making the program coordinates of the top of the work be zero as is conventional for most
programs.
Figure 6.9 shows the top of the table as being machine
zero. This is arbitrary. We could have chosen the top
face of the stand and the diagram would have looked
very similar – just that the work offset and machine
coordinates for the given head position would have been
bigger.
In practice the zero position of the referenced machine
is chosen to be where the head stops after clicking Ref
Z i.e. just below the Z limit/home switch (figure 6.10).
This means that in normal use all Z machine coordinate
values will be negative numbers and the work offset
values will be negative too. The arithmetic of the
equation
Figure 6.10 – Actual machine zero
Program Coordinates + Work Offset + Tool Length = Machine Coordinates
works fine with the negative values but it is not possible to draw a simple sketch like figure 6.9.
The fact that machine zero can be anywhere and the work offset relates it to the work location
explains why it is possible to use the machine un-referenced. In this case machine zero can be
anywhere; below the floor, up in the roof space, etc. The work offset value when you have
touched the tool on the top of the work will make this position be program coordinate Z = 0.0.
6.2.3
Programming, Buttons, or Direct Entry
The example above shows the tool being selected directly through typing a number into the tool
DRO.
32397 Rev C1-2
6-5
Using Tormach PCNC 1100 Series 3
Offsets
You can also command the tool change by entering directly into the MDI line. Specifically
when switching to tool number n, enter Tn M6 G43 Hn on the MDI line. M6 is the
command to do a tool change and T indicates the tool number to use. G43 says that a tool
length offset must be be applied with H giving the offset length to use – this is usually the same
as the number of the tool you have chosen. As an example, if you want to change to tool #21,
the command would be:
M6 T21 G43 H21
If you're creating a G&M code program by hand, in a text editor, this sort of line will be needed
when your code intends to command a switch from one tool to the next. If you develop your
code using a CAM program, your CAM program will automatically insert this line.
6.3
Alternative Methods Setting Up Tools
The previous section showed you how to measure tools and set up the tool table if you have the
Tormach Tooling System (TTS) and its touch tool. Working this way is easy to explain and
understand as well as allowing you to set up tools for the next job while using the machine to
run a job. Offline measurement is common in professional toolrooms but TTS is one of the few
systems making it available to small ‘shops.
This section describes ways of using the mill itself to measure tools and is applicable to
standard R8 tooling which is difficult to measure offline.
It can, of course, also be used with TTS if you do not wish to measure offline. You must
however be consistent with the method you use. You cannot measure some tools offline and
some online. The reason for this is that any measurement is based on a reference or datum
position. In TTS the datum is the cylindrical ground spacing piece in which the tools stand.
When measuring online you have to consider one of your tools to be the reference or “master”
tool.
6.3.1
Measuring techniques
Now it is time to go from the theory of
coordinate systems to the very practical
choice of the best ways of finding where
a tool is in relation to stock which you
want to machine. We will look at ways of
measuring tool position and then how you
use these measurements to set up the
PCNC.
We will concentrate for the present on the
position of the Z-axis. There are several
reasons for this:
•
Figure 6.11 – "Roll-your-own" gauge in use
The Z dimension is often the one
with the highest accuracy
constraints because the stock is often oversize in both dimensions in X and Y and is, at
any event, not easy to locate precisely on the table.
•
The Z direction is not only important for setting the initial position of the stock it needs
to be accounted for when using several tools which are, almost inevitably, of different
lengths.
Note: We assume that the top surface of your work-piece is the plane Z = 0.0.
Using Tormach PCNC 1100 Series 3
6-6
32397 Rev C1-2
Offsets
6.3.1.1
“Roll-Your-Own” Gauge Method
This is a time honored machinists’ method
which traditionally used Rizla or similar
cigarette paper as a gauge. The plastic foil
from candy wrapping is a good substitute.
Both materials are fairly strong and around
0.002" in thickness.
Jog the tool very carefully down to the
stock with a piece of paper/foil on it (figure
6.11). You will be able to feel when the
paper/foil gets trapped.
You then know that the tool is 0.002” (two
“thou”) above the stock.
The advantage of this method is that you
will always be able to “find” a gauge and it
can be used on a very small flat surface on
the stock (e.g., the boss of a casting). The
disadvantage, particularly with hard stock
and brittle tools (e.g., carbide) is that it is
easy to jog down too far and damage the
tool cutting edge.
6.3.1.2
Figure 6.12 – Tool much too low for gauge
Roller Gauge Method
For this method you need a short length of
rod of a known diameter (¼" is quite
suitable for most jobs). The shank of a
twist-drill can be used in an emergency but
take care to use one without scoring on it
and measure the diameter rather than
assuming it is the nominal size of
the drill.
Figure 6.13 – Gauge just rolls under tool
Jog the tool so it is clear of the
stock but no more than the gauge
diameter above it. You will be
unable to roll the gauge under the
tool (figure 6.12). While
attempting to roll the gauge into
the gap, very slowly jog upwards.
You will easily feel the point
where the gauge rolls under (figure
6.13). If you jog too far then it is
easy to remove the gauge, jog
down a little and try again.
You know that the tool is the
diameter of the gauge above the
stock.
Figure 6.14 – Parallel adjusted to gap
The advantages of this method are that you do not risk crashing the tool into anything. If you
are repeatedly gauging, (say multiple tools) then you do not have to keep typing a measurement
into the Control Program. One disadvantage is that any backlash in the Z axis will cause an
error as you are jogging on the other side of the backlash from that when a cut has been applied.
You also need to be able to jog slowly to get an accurate result. The Jog/Shuttle device is very
convenient on account of its variable jogging speeds..
32397 Rev C1-2
6-7
Using Tormach PCNC 1100 Series 3
Offsets
6.3.1.3
Adjustable Parallel Method
You need an adjustable sliding parallel
gauge.
Jog by eye so that the tool is about the
nominal size of the parallel. Insert it in
the gap between tool and stock, slide it
to fill the gap and lock it off (figure
6.14).
Carefully remove the parallel and
measure it with a micrometer or caliper
(figure 6.15).
The advantage of this method is that you
do not need any careful jogging. The
Figure 6.15 – Measuring the parallel gauge
disadvantages are the need to measure
the parallel and then to accurately type
the result, which will generally be an awkward number, into the DRO.
You can of course use a combination of these methods depending on what you have to hand on
a job and which is most convenient.
6.3.2
Comments on Accuracy
With practice you will be able to use these methods to measure to better than 0.001". It is,
however, interesting to look at other issues which affect the accuracy of your work.
The PCNC is a rigid machine and is fitted with precision anti-backlash ballscrews and laser
aligned in the factory so is inherently very accurate. You do however need to consider the
following points:
•
You are measuring at one point on the stock. If its surface in not flat or it is not
clamped exactly parallel to the table then the height at other places will be different.
•
A change of 40oF in the temperature of a ballscrew (say between early morning in the
winter and when the shop and machine has heated up in the afternoon) will amount to a
difference of around 0.004" when the tool is near the table at the bottom of the Z-axis.
General Accuracy Issues
Machining is a mix of science, skill and art. The caveat in stating accuracy and repeatability is
that these factors depend on the techniques used by the machinist. A skilled machinist can often
deliver accuracy that exceeds the accuracy specified by the machine builder, while an
inexperienced machinist may have difficulty delivering the expected accuracy. With this
understanding, we cannot tell you what accuracy you will be able to achieve in your own work.
While a machine tool may seem absolutely rigid, the truth of the matter is that everything has
some elasticity. Related to elasticity is the compressibility of components such as ball nuts and
bearings. Preloading of bearings and ballscrews can remove the physical open space between
moving parts, but the technique cannot eliminate compressibility. The key to achieving
maximum accuracy is understanding and controlling the magnitude and direction of forces.
Maximum accuracy is achieved when the forces are minimized, as occurs in a finishing cut.
Maximum repeatability is achieved when the forces are repeatable, both in magnitude and
direction.
6.3.3
Working without the tool table
You do not need to use the tool table.
If you hold your tools by a method which does not give a consistent length (e.g. exchanging
tools in a collet) then you will not be able to use a tool table.
Using Tormach PCNC 1100 Series 3
6-8
32397 Rev C1-2
Offsets
If you have work which is generally one-off and you use a very wide range of tools (e.g. many
different drill diameters) then it is probably not worth the trouble of setting up the tool table.
To work without a tool table you merely reset the Z axis work offset value each time you
change the tool.
6.3.3.1
Direct Entry to Axis DRO
All the measurement methods give the current
position of the tool relative to the stock,
assuming the face you have measured to is to be
zero in the program coordinates, all you need to
do is to type the value into the relevant axis
DRO. You can do this on any screen.
For example after using the adjustable parallels
(figure 6.15) and without moving the axis, you
would enter 0.547 into the Z-axis DRO (figure
6.16).
Figure 6.16 – Gauge size entered to DRO
The program coordinates say Z = 0.547 and the tool is 0.547" above the stock so, for example,
G00 Z0.0 will move the tool so it exactly touches the stock.
You may have noticed that in making FirstPart we cheated a little by assuming the paper
gauge was zero thickness. This is often sufficiently accurate and allows use of the Zero buttons
rather than typing a value.
6.3.3.2
Using the Touch Buttons
The “roll-you-own” and roller gauge methods
will always give you the same measurement
to be typed in. On the Offsets screen you can
do this once and use it each time you want to
set-up an offset.
The gauge thickness is typed into the Touch
Correction DRO on the Offsets screen. Figure
6.17 shows this being set for the ¼" roller
gauge. Note the correction is also enabled as
shown by the LED by the On/Off button.
Figure 6.17 – Entering roller gauge size
When the gauge is in place, clicking the
Touch button for the axis will set the offset. Figure 6.18 shows the program coordinates after
Touch on Z-axis.
Figure 6.18 – Touch done on Z with roller gauge
32397 Rev C1-2
6-9
Using Tormach PCNC 1100 Series 3
Offsets
6.3.4
Tool Table with General Tooling
With conventional tool holders you will not be able to
measure them with a height gauge (unless, of course, you
make your own dummy R8 spindle nose). The following
procedure uses the PCNC as a measuring rig.
Note: If you follow these instructions very carefully you
can mix tool entered into the tool table by measuring on
the TTS granite block with those measured in the
machine. We suggest, however that you do not mix the
two methods. If you want to use TTS and R8 tools on a
job the just measure all of them on the machine as
described below.
Mount a piece of flat stock on the table or in a vise on the
PCNC. Work throughout on the Offsets screen.
If you have some TTS tools preset in the tool table then
one of these must be the master tool. If you have R8
tooling choose one that you do not expect to wear much
in use to be tool #1. This is termed the master tool
Load the master tool, select tool #1 (or tool #0 if you have
a non-cutting master) in the T DRO. If it is a TTS tool and
so already in the table then its length should be shown as
in the Length DRO. If it is not in the table them
type 0.0 in the Length press Enter to accept it.
Figure 6.19 – Setting up a
conventional
tool holder as tool #4
Now set the work offset with it touching the work to
Z = 0.0 by any of the gauging methods described
above.
Now jog the Z-axis so you can load each tool holder
in turn. Enter its number into the T DRO. Jog and
gauge (by any of the touching methods already
used) but instead of entering the gauged position
into the Z-axis DRO you must always enter it into
the Touch Correction DRO and click the tool Touch
button marked Length – not any of those in the
Work Offsets column. For completeness, enter the
diameter of the tool in the Tool Diameter DRO. Do
not forget that you have to press Enter to accept
values typed into DROs.
Figure 6.20 - Toolsetter
What you are doing is setting the lengths of all the tools relative to the Master Tool.
Figure 6.19 shows this having been done for tool #4.
6.3.5
Tool table with the Tool Setter
If you have the Tormach Tool Setter then this can easily be used to set entries in the tool table.
Details are given in Chapter 8 (figure 6.20).
6.4
Comments on Tool Offsets
If you do not save the Tool Table then, when you close down the Control Program, you will be
asked if you want to save it. Unless you have made a serious error in setting up tool offsets you
should save them or you will have to enter them again next time you run the Control Program.
Using the T DRO on a screen is a very easy way of changing a tool. The process is more
complex in a part-program. This is because the RS-274 standard part-programs can run on large
Using Tormach PCNC 1100 Series 3
6-10
32397 Rev C1-2
Offsets
CNC systems with complex automatic tool changers. The RS-274 process consists of choosing
the next tool to use with a T word, Loading the tool with M06 and applying its offsets with
G43. The required commands will be generated by CAD/CAM systems and the Wizards. We
strongly advise you to put all three stages (T~, M06 and G43 H~) on one line in you program
and to check that the post processor of your CAM system does this. If you do not follow this
"Triplet Rule" then you will encounter problems if you mix using tool lengths in the tool table
and just setting the work offset when you change a tool.
6.5
Setting X and Y Offsets
The X and Y offsets allow the actual position of you work on the table to be converted to the
machine coordinates whenever a movement is required. It is usual to the top left coner of the
work-piece to be used in the G-code as X = 0.0, Y = 0.0. If your code uses another convention
then set 0, 0 to the place used in your code.
6.5.1
By eye
It is sometimes quite acceptable to define the program
coordinate zeros by eye as was done for
FirstPart.
Move the tool to be above the point you want to be X
= 0.0 and click the Zero button by the X axis DRO
(on any screen). Now move the table so the tool
centre is above the position to be Y = 0.0 and click
Zero by the Y axis DRO. You can if you prefer just
type 0 (followed by Enter) into the DRO and Y = 0.0
and
There are useful techniques when more accuracy is
required.
6.5.2
With a Probe
By far the most accurate and often the quickest way of
setting X and Y offsets to a piece of stock material or
to a part-machined component is with a probe such as
that illustrated in figure 6.21 Full details of the
support for this accessory are given in chapter 8.
6.5.3
Figure 6.21 – The Tormach probe
Measuring Off an Edge
Any of the above gauge methods can be
used with a “tool” touching the edges of
the stock or equally usefully the jaws of a
vise used to hold the stock.
It is not really practicable to use a cutter
because the spiral flutes do not give a clear
place to gauge to. A cylindrical bar (e.g.,
½" diameter) is ideal. It should be mounted
in a tool holder so that it runs true. It is
slightly easier to feel the contact point if a
spherical finder is used. This is shown in
the illustrations below.
Figure 6.22 show the measurement of the
coordinates on the corner of the fixed jaw
of a machine vise.
32397 Rev C1-2
6-11
Figure 6.22 – Measuring vise jaw Y position
Using Tormach PCNC 1100 Series 3
Offsets
The value to be use in the Touch
Correction DRO (or entered in the axis
DRO) is half the diameter of the probe
tool plus the measurement of the gauge.
In the illustrated setup the ball has a
diameter on 0.369" so with 0.002" foil the
correction is numerically -0.1865".
The same technique can obviously be
used on the edges of a piece of stock
clamped to the table.
Figure 6.23 – “Inside” corrections are negative
Note: You need to be careful about
whether the correction is plus or minus. In
the case of the vise jaw it is negative (the
center of the tool is actually nearer to 0.0
that the touching point). For the outside of
a workpiece it should be positive. Thus in
the example illustrated, the value typed
into the Touch Correction DRO will be 0.1865 (figure 6.23).
6.5.4
Laser Centering Techniques
If you need to setup the X and Y program
coordinates to features marked on, or
already machined in, the workpiece then a
laser finder or centering microscope is
very useful.
Figure 6.24 shows a laser finder located
near a center-punch mark on the stock.
The point of light can be more clearly seen
in the close-up view (figure 6.25)
Viewing the feature through a centering
Figure 6.24 – Laser finder on scribed mark
microscope has the same effect although
the height of the Z-axis is then much more important as it affects the focusing of the
microscope.
Obviously no correction is needed for the position as the beam is where the center of the tool
will be.
6.6
How Work Offsets work
We have shown you several uses of offsets.
This section gives a summary of how they
work internally.
As explained above the PCNC keeps track of
the absolute position of all axes. If it has
been referenced then these will be
measurements relative to the home switches
on the X, Y and Z axes. It it has not been
referenced then the machine coordinates will
be arbitrary.
Machine coordinates are useless for
programming the machine as you will not
Using Tormach PCNC 1100 Series 3
6-12
Figure 6.25 – Close-up of spot of light
32397 Rev C1-2
Offsets
know when designing a part what they will be at a datum position (e.g. one corner of the part.
This is why you define a relation between the Program Coordinates and Machine Cordinates..
Figure 6.26 – Illustrating Program and Machine coordinates
This relationship is just a series of Offsets. The offsets are numbers which are added by the
Control Software to your program X, Y, Z coordinates to get the machine coordinates.
Figure 6.26 is a view of part of the Offsets
screen. You will probably find it useful to look
at this screen on your machine as you read this
material. The machine is set-up in Inch
(imperial units). If your machine is set-up for
metric units then you can either experiment
with the same numbers as we use or, of course,
roughly convert them to inches
To obtain figure 6.26 the PCNC was referenced
(notice the green “referenced” LEDs at right of
screen) and a tool jogged to the surface of a
Figure 6.27 – Axis DROs corresponding to
figure 6.26
piece of stock just touching the surface at the
top left corner. So you can imagine it, let us say
that the jogging moved the Z-axis down about 9.5", the tool 3" to the right and 2.5" towards the
front of the machine.
The Zero button for X-, Y- and Z-axes was clicked (we could have typed 0 into the axis DROs
with exactly the same effect). The Manual Data Input (MDI) was then used to go to the
program coordinate position X = 1, Y = -1.4 and Z = 0.5 by:
G00 X1.0 Y1.4 Z0.5
Figure 6.27 shows the axis DROs that you would see, while the whole story is shown in figure
6.26. Let us use X as an example. The program coordinate for the tool is currently X= 1.0 (we
did a G00 X1.0). The offset to be added to this to get the machine coordinate is 3". Adding
these two values together gives the machine coordinate value of 4. These numbers are nice
round values in practice if you jogged exactly to the top left corner of the stock they will have a
decimal fraction part (e.g. 9.076).
Now look at Z. The jog was about 9.5" down but we put the tool exactly on the surface of the
stock. The program coordinate is Z = 0.5 (from the G00 Z0.5). The Z offset value is actually
-9.5. Adding the program coordinate to the offset gives the machine coordinate of -9.0. This is
of course the distance that the head currently is below the home switch position. It may seem
strange at first when you have negative numbers. All you have to remember is that a sum:
4.3 + (-2.1) is identical to 4.3 – 2.1
The offsets we have been setting are called Work Offsets as they are different for each piece of
work loaded onto the machine. The Z offset includes the length of the tool. If you change the
tool then you would have to jog so the new one is just touching the work and click Zero again.
32397 Rev C1-2
6-13
Using Tormach PCNC 1100 Series 3
Offsets
In the next section we will see how another sort of offsets, Tool Offsets, can allow for the
different projection of different tools from the spindle nose.
You are probably wondering how you can jog so that the spindle axis (i.e. the centre of the tool)
is exactly over the corner of a work-piece (to set X = 0.0 and Y = 0.0) and how to safely lower
the tool to the top of the work to get Z = 0.0. There are many possible techniques some of
which are explained later in this chapter.
Although we Referenced the machine so machine coordinates are zero at the home switch
position this is not essential. Clicking the Zero button on axis DROs will set a work offset value
whatever the value of the machine coordinates.
So to summarize, any move made in a part-program or by typing in the MDI line which gives a
new set of program coordinate values will cause the Control Software to add on the appropriate
offsets and then move the machine position to the newly calculated value of the machine
coordinates value. The sum it does is shown on the Offsets screen.
You may find it helpful to move the tool around on your machine above some scrap stock and
use a tape-measure to reconcile the DRO readings with the machine position relative to the
switches and the stock. When you have a clear picture in your mind of what is happening you
have mastered the idea of offsets and should have no problems with this chapter.
6.7
Multiple Work Origins
6.7.1
G54 Work Offset
The previous explanations of offsets have only referred to a single set (X, Y, Z, A) of work
offsets. These are always in effect when the Control Software is loaded.
It is sometimes useful to have another set of offsets and for them to be persistent when the
system is closed down and reloaded. Suppose you have a machine vice permanently fixed to the
table. It would be useful to remember the top left corner of its fixed jaw as this is a simple
datum to locate stock.
6.7.2
Other Work Offsets
The control software allows you to setup a total of more
than 250 different sets of work offsets; most people will
only use the first six as these are easily selected using the
codes G54 to G59. The Offsets screen has a pair of buttons
to select the work offsets that are in use and displayed
(figure 6.28).
When you Touch or enter values in the axis DROs then you
will update the current set of work offsets.
You can save the work offset values using the Edit/Save
table Now button above the Work Offset DROs. This button
displays the complete table. It can be edited manually and is
saved by clicking the Save button. The dialog is closed by
clicking OK.
If you do not save the work offset table then, when you
close down the Control Program, you will be asked if you
want to save it. Unless you have made a serious error in
setting up work offsets, you should save them or you will
have to enter them again next time you run the Control
Program. We advise you not to alter the G54 offsets
although it is remembered from run to run of the Control
Software.
Using Tormach PCNC 1100 Series 3
6-14
Figure 6.28 – Choosing
Work Offsets
32397 Rev C1-2
Offsets
6.8
Cutter Diameter Compensation
6.8.1
CAD/CAM and Wizards
We have shown how it is necessary to allow for the diameter of the tool when cutting around an
object or cutting out a pocket. You are strongly advised to do this by your CAD/CAM software
or the Wizard which generates the part-program. The advantage of it being done this way is that
the software has knowledge of the future path of the tool so can avoid overshooting on sharp
inside corners. In general this cannot be done by the control software.
Some systems allow code written by hand of by CAM to be fine tuned when it is run by
adjusting the diameter of the cutter. We advise against trying to do this with the current version
of the Control Software. Generate code by using CAM or writing by hand to move the centre of
the cutter along the path that will give you the cut you require with the planned diameter of
cutter. In other words, avoid the use of G41 or G42 commands.
You are unlikely to need to read the remainder of this chapter which describes the actual
operation of the Control Software.
6.8.2
Concepts for Cutter Diameter/Radius Compensation
The standard mode is for cutter compensation to be off (G40). Without cutter compensation the
machine will follow a tool path that is defined by the G- code program. With cutter
compensation turned on (G41, G42) the actual path the machine follows will be offset, left or
right of the stated path, by an amount specified in the tool offset table.
There are two ways to use cutter radius compensation. The most obvious way is to have the
offset stated in the tool table to be the diameter of the tool. In theory this would allow the Gcode program to simply define the geometry of the actual part to be machined with the machine
controller left to calculate the tool paths necessary to compensate for cutter diameter. In
practice the problem is far more complex and can lead to a great deal of trouble in debugging
the G-code program.
Another way to use cutter compensation is as a small
correction factor, where the tool path planning is done
outside of the machine and the offset is used to only to
make minor adjustments. This approach can be used to
make fine adjustments for tool wear, part tolerance, or
final finish cuts for rough cutting to finish cutting.
6.8.3
Caveats in the Use of Cutter Compensation
While the concept has useful applications, there are
many pitfalls in actual practice. This is not a
programming technique for beginners. A few of the
issues are listed below:
1. Proper application is complex and involves a
large number of coding specific rules. The most
complete reference we know of is A
Comprehensive Guide to Practical CNC
Programming2 in which the author describes
how to apply radius offsets in 24 pages of the
book.
Wear Compensation Example
Suppose a shop prefers to resharpen
cutting tools, not disposing of a tool
until it is more than 0.005” reduced
in diameter. In this situation a
programmer could do his CAM
work and create a G & M code with
a tool path that assumes a 0.495”
diameter for a 1/2” diameter tool.
When the tool is new and has a true
0.500” diameter, the operator will
put 0.005” in the offset table for the
tool (0.495 + 0.005 = 0.500). As the
tool is sharpened and becomes
smaller, the offset is appropriately
reduced. When the offset needed is
zero, the tool is replaced. Using this
approach the operator can us both
new and resharpened tools with the
same G&M code program.
2. Path planning is highly sensitive to lead in and
lead out planning. The machine controller cannot compensate under all conditions.
2
A Comprehensive Guide to Practical CNC Programming (ISBN 978-0-8311-3347-4) by Peter Smid is one of
several advanced machining and programming books available from the Tormach web site (www.tormach.com).
32397 Rev C1-2
6-15
Using Tormach PCNC 1100 Series 3
Offsets
3. There is no truly standard implementation of cutter compensation. If you have
experience in using cutter compensation with Fanuc, Siemens, GSK, Haas, Centroid, or
other control systems, do not expect the Mach3 implementation to react in the same
manner.
4. Utility and application may be limited by the look-ahead limit. Cutter compensation in
Mach3 cannot prevent clipping corners when going into internal cavities. See the
example in section 6.6.4.
5. Mach3 has limitations in scope of application of cutter radius compensation. We
advise against using cutter compensation in combination with subroutine programming,
canned cycles, macro programming, polar mode, with run from here function, and with
multiple work offsets.
The complexity of application for cutter compensation can lead to hours of programming
debugging. Given the nature of the problem, Tormach cannot provide program debugging
support nor resolve application specific questions regarding the use of cutter compensation.
6.8.4
Examples of Operation
The program below plans cutting a rectangle which is 2” x 2”. The graphic below shows two
paths. On the left, in a solid line, we see the path described by the G code program. On the
right, in the dashed line, we see the actual path that is followed by the Mach3 controller when
tool #1 is programmed with a 0.5” diameter.
G Code Path
Actual Tool Path with
Cutter Compensation
(begin at X1.50, Y-1.25)
(begin at X1.50, Y-1.25)
(end at X1, Y-1.5)
(end at X1.25, Y-1.5)
Figure 6.29 – Toolpath in Example 1
Example 1:
G17 G20 G40 G49 G50 G64 G90 G94
M6 T1 G43 H1 (Select Tool 1 and offset 1)
G0 Z1 M3 S1000 (Start Spindle)
X1.5 Y-1.25 (Move to lead in position)
G1 z-.5 f50 (Z down to cutting level)
G41 (Turn on cutter compensation)
G1 X1 Y-1 (Cut around block which is 2x2 in dimension)
X-1 Y-1
X-1 Y1
X1 Y1
X1 Y-1.5
G40
G0 X 1.5 Y-1.5 Z1 M5(Z up, spindle off)
Using Tormach PCNC 1100 Series 3
6-16
32397 Rev C1-2
Offsets
The result of the offset is that the planned 2”x 2”
block is cut out. A composite drawing, figure 6.30,
shows this along with the tool diameter.
Now let’s look at a slightly different example to see
what can go wrong. The example below is nearly
identical, but a slightly different starting point is used
which is 0.25” lower in Y. At first glance it seems
fine.
(begin at X1.50, Y-1.25)
Example 2:
(end at X1.25, Y-1.50)
Figure 6.30 – Example 1 overlaid
G17 G20 G40 G49 G50 G64 G90 G94
M6 T1 G43 H1 (Select tool1)
G0 Z1 M3 S1000 (Start Spindle)
X1.5 Y-1.5 (position above lead in point)
G1 z-.5 f50 (Z down to cutting level)
G41 (turn on cutter compensation)
G1 X1 Y-1
X-1 Y-1
X-1 Y1
X1 Y1
X1 Y-1.5
G40
G0 X 1.5 Y-1.5 Z1 M5
M30
Actual Tool Path with
Cutter Compensation
G Code Path
(begin at X1.50, Y-1.50)
(begin at X1.50, Y-1.50)
(end at X1.25, Y-1.50)
Figure 6.31 – Toolpath in example 2
The coded path and resulting compensated tool look
similar, but the lead in here is coming in at a 45 degree
angle.
Looking at the combined result (figure 6.32) we what
might seem correct.
(begin at X1.50, Y-1.50)
(end at X1.25, Y-1.50)
Figure 6.32 – Example 2 overlaid
32397 Rev C1-2
6-17
Using Tormach PCNC 1100 Series 3
Offsets
But when we take a closer look at the
first corner we can see that the lead in
came a bit short, leading to a burr on the
corner. An adjustment of the initial lead
in position is necessary to fix this.
Detailed issues like this are difficult to
find in advance, which is one of the
reasons that use of cutter compensation
can be time consuming to debug.
Programming of entry moves is critical
when using cutter compensation and
some debugging of a program is
frequently necessary.
Figure 6.33 – Detail of example 2
Programming Entry Considerations
In general, an alignment move and two entry moves are best to begin compensation correctly.
However, where the G41/G42 compensation is only going to be used as a small correction
factor, it’s usually possible to incorporate only one entry move (plus, possibly, a pre-entry
move) is needed. The general method, which will work in most situations, is described first. We
Figure 6.34 – General Entry Move solution
Using Tormach PCNC 1100 Series 3
6-18
32397 Rev C1-2
Offsets
assume here that the programmer knows what the contour is already and has the job of adding
entry moves.
General Method
The general method includes programming an alignment move and two entry moves. The entry
moves given above will be used as an example. Here is the relevant code:
G1 X1 Y4.5 (make alignment move to point C)
G41 G1 Y3.5 (turn compensation on and make first entry
move to point B)
G3 X2 Y2.5 I1 (make second entry move to point A)
Figure 6.34 shows the two entry moves but not the alignment move. First, pick a point A on the
contour where it is convenient to attach an entry arc. Specify an arc outside the contour which
begins at a point B and ends at A tangent to the contour (and going in the same direction as it is
planned to go around the contour). The radius of the arc should be larger than half the diameter
given in the tool table. Then extend a line tangent to the arc from B to some point C, located so
that the line BC is more than one radius long. After the construction is finished, the code is
written in the reverse order from the construction. Cutter radius compensation is turned on after
the alignment move and before the first entry move. In the code above, line N0010 is the
alignment move, line N0020 turns compensation on and makes the first entry move and line
N0030 makes the second entry move.
In this example, the arc AB and the line BC are fairly large, but they need not be. For a toolpath
contour, the radius of arc AB need only be slightly larger than the maximum possible deviation
of the radius of the tool from the exact size. Also for a toolpath contour, the side chosen for
compensation should be the one to use if the tool is oversized. As mentioned earlier, if the tool
is undersized, the interpreter will switch sides.
6.8.5
Look Ahead Issues
There can be problems with cutter compensation related to the lack of foresight on the part of
the controller. The program below plans cutting an edge using cutter compensation shown in
the graphic as CDEFGHIJ. The segments AB and BC are entry segments as described above.
G17 G20 G40 G49 G50 G64 G90 G94
M6 T1 G43 H1
G0 X-1 Y2 Z1 M3 S1000 (position above starting point)
G1 z-0.5 f50 (Z down to cutting height)
G41 X-1 Y1 (Making the first entry move to point B)
G3 X0 Y0 R1 (Doing the entry arc to point C)
G1 X1 (cutting to point D)
Y-1.5 (cutting to point E)
X2 (cutting to point F)
Y-0.5
X1.5
Y0
X3.5
G40
G0 Z1 M5
M30
In figure 6.35 we can see how a 1/4” tool will cut this. The process is successful, but only
because of the small diameter of the cutter.
32397 Rev C1-2
6-19
Using Tormach PCNC 1100 Series 3
Offsets
A
B
C
J
I
H
D
E
G
F
Figure 6.35 – Compensating a small tool
If we change to a 0.787” cutter (common 20 mm end mill) we see the results in figure 6.36.
A
B
C
J
I
H
D
E
G
F
Figure 6.36 – Compensation fails with large tool
Using Tormach PCNC 1100 Series 3
6-20
32397 Rev C1-2
Offsets
What has happened here is that the cutter is too big for the channel in the pocket. As it is cutting
path DE, it’s removing the sidewall of IH. Likewise on the way out, it will destroy a segment
of wall DE while it climbs out along path IH. We would prefer that the controller would either,
1) stop and generate an error message, or 2) cut a path from D to I, avoiding the cavity created
by EFGH. That’s not what happens. This type of error is less common when doing cutter
offsets and exact path planning in your CAM software as opposed to using the controller to
calculate offsets.
6.8.6
Other Restrictions
•
All moves should be longer than the amount to be offset. This restriction makes it clear
the increased limitations of using cutter compensation to offset for the full tool radius
instead of using it to only compensate for wear, tolerance, or final finish depth of cut.
•
Leadin moves should be longer than the amount you want to offset.
•
The radius of an inside arc should be greater than that of the cutting tool.
•
The Mach3 tool table includes both Diameter and Diameter Wear columns. Always use
the Diameter column, even when only using G41/G42 for wear compensation. The
Diameter Wear data column in the Mach3 tool table is for future development and does
not function as of this writing.
•
There must not be more than 50 consecutive lines of code without a movement
command, e.g. XY positions only.
•
Cutter compensation must not be applied or canceled on a G02 or G03 command. A
legal line would be:
G01 G42 P2.5 X20 (legal)
G02 G42 P2.5 X20 Y0 R10 (illegal)
6.8.7
Perspective on Cutter Compensation
In the past, effective and affordable CAM software was simply not available and, despite all the
pitfalls and complications, application of G41/G42 cutter compensation in a CNC machine tool
was more common. There was simply no other solution. Now that high quality CAM software
is widely available most people do tool offsets in CAM and don’t bother with using G41/G42
for offsets in the machine controller.
Nevertheless, there remain instances where controller based offsets are useful. If you decide to
use the G41/G42 codes, be prepared for considerable debugging. Some apparent roadblocks
may be avoided through experimentation and minor modifications to your G-code program.
Others may be inherent to Mach3 or the desired geometry you are trying to achieve.
As a matter of practical experience, we recommend path planning in CAM and avoiding the use
of G41/G42 where possible. When it becomes necessary to us the G41/G42 functions we
suggest you apply the codes to simple geometry parts, applying small compensations (i.e. wear
compensation, not cutter radius compensation), using 2 segment lead in, and be prepared for
some experimentation/debugging.
6.8.8
Resources for Debugging Cutter Compensation
As noted earlier, Tormach cannot provide program debugging support nor resolve application
specific questions regarding the use of cutter compensation. Basic solutions for debugging
code files can usually be resolved through a systematic approach of “divide and conquer”,
where you section codes and single step through a code, sometimes in combination with M1
optional stop statements. Additional guidance can be had from:
Programming of CNC Machines, by Ken Evans. Refer to section 4 pages 250 to 261
32397 Rev C1-2
6-21
Using Tormach PCNC 1100 Series 3
Offsets
CNC Programming Techniques, by Peter Smid. Refer to chapter 4, pages 46 to 66
Both of these reference books are available through the Tormach web site (www.tormach.com)
Final Note: We should re-iterate that it is much better for a CAM program to generate the path
of the tool allowing for its diameter because it can "see" the implications of cutting complex
corners in a way which the control software cannot.
Using Tormach PCNC 1100 Series 3
6-22
32397 Rev C1-2
Programming language reference
7.
Part-programming Language Reference
This section defines the language (G-codes, etc.) that are understood and
interpreted by the Control Software.
This chapter is intended for reference purposes. Sample programs using these
commands are included in the folder C:/PCNC3/GCode.
If you want to learn about the principles of the control language so you can write
programs by hand from first principles then you should consult an introductory
textbook on G-code programming.
7.1
Definitions
7.1.1
Control Software
This is the term used for the program running under Microsoft Windows in the PC connected to
your PCNC. In this chapter the Control Software is shortened to the CS.
7.1.2
Linear Axes
The X-, Y- and Z-axes form a standard right-handed coordinate system of orthogonal linear
axes. Positions of the three linear motion mechanisms are expressed using coordinates on these
axes.
7.1.3
Rotational Axes
The rotational axes are measured in degrees as wrapped linear axes in which the direction of
positive rotation is counterclockwise when viewed from the positive end of the corresponding
X-, Y- or Z-axis. By “wrapped linear axis,” we mean one on which the angular position
increases without limit (goes towards plus infinity) as the axis turns counterclockwise and
decreases without limit (goes towards minus infinity) as the axis turns clockwise. Wrapped
linear axes are used regardless of whether or not there is a mechanical limit on rotation.
Clockwise or counterclockwise is from the point of view of the workpiece. If the workpiece is
fastened to a turntable which turns on a rotational axis, a counterclockwise turn from the point
of view of the workpiece is accomplished by turning the turntable in a direction that (for most
common machine configurations) looks clockwise from the point of view of someone standing
next to the machine.
7.1.4
Scaling Input
It is possible to set-up scaling factors for each axis. These will be applied to the values of X, Y,
Z, A, I, J and R words whenever these are entered. This allows the size of features machined to
be altered and mirror images to be created – by use of negative scale factors.
The scaling is the first thing done with the values and things like feed rate are always based on
the scaled values.
The offsets stored in tool and fixture tables are not scaled before use. Scaling may, of course,
have been applied at the time the values were entered (say using G10).
32397 Rev C1-2
7-1
Using Tormach PCNC 1100 Series 3
Programming language reference
7.1.5
Controlled Point
The controlled point is the point whose position and rate of motion are controlled. When the
tool length offset is zero (the default value), this is a point on the spindle axis (often called the
gauge point) that is some fixed distance beyond the end of the spindle, usually near the end of a
tool holder that fits into the spindle. The location of the controlled point can be moved out
along the spindle axis by specifying some positive amount for the tool length offset. This
amount is normally the length of the cutting tool in use, so that the controlled point is at the end
of the cutting tool.
7.1.6
Coordinated Linear Motion
To drive a tool along a specified path, a machining system must often coordinate the motion of
several axes. We use the term “coordinated linear motion” to describe the situation in which,
nominally, each axis moves at constant speed and all axes move from their starting positions to
their end positions at the same time. If only the X-, Y- and Z-axes (or any one or two of them)
move, this produces motion in a straight line, hence the word “linear” in the term. In actual
motions, it is often not possible to maintain constant speed because acceleration or deceleration
is required at the beginning and/or end of the motion. It is feasible, however, to control the axes
so that, at all times, each axis has completed the same fraction of its required motion as the
other axes. This moves the tool along the same path and we also call this kind of motion
coordinated linear motion.
Coordinated linear motion can be performed either at the prevailing feed rate or at rapid
traverse rate. If physical limits on axis speed make the desired rate unobtainable, all axes are
slowed to maintain the desired path.
7.1.7
Feed Rate
The rate at which the controlled point or the axes move is nominally a steady rate which may be
set by the user. In the Interpreter, the interpretation of the feed rate is as follows unless inverse
time feed rate (G93) mode is being used:
7.1.8
•
For motion involving one or more of the linear axes (X, Y, Z and optionally A, B, C),
without simultaneous rotational axis motion, the feed rate means length units per minute
along the programmed linear XYZ(ABC) path.
•
For motion involving one or more of the linear axes (X, Y, Z and optionally A, B, C), with
simultaneous rotational axis motion, the feed rate means length units per minute along the
programmed linear XYZ(ABC) path combined with the angular velocity of the rotary axes
multiplied by the appropriate axis Correction Diameter multiplied by pi, where
π = 3.14152 (i.e., the declared “circumference” of the part).
•
For motion of one rotational axis with X-, Y- and Z-axes not moving, the feed rate means
degrees per minute rotation of the rotational axis.
•
For motion of two or three rotational axes with X-, Y- and Z-axes not moving, the rate is
applied as follows: Let dA, dB and dC be the angles in degrees through which the A-, Band C-axes, respectively, must move. Let D = sqrt (dA2 + dB2 + dC2). Conceptually, D is a
measure of total angular motion, using the usual Euclidean metric. Let T be the amount of
time required to move through D degrees at the current feed rate in degrees per minute. The
rotational axes should be moved in coordinated linear motion so that the elapsed time from
the start to the end of the motion is T plus any time required for acceleration or
deceleration.
Arc Motion
Any pair of the linear axes (XY, YZ and XZ) can be controlled to move in a circular arc in the
plane of that pair of axes. While this is occurring, the third linear axis and the rotational axes
can be controlled to move simultaneously at effectively a constant rate. As in coordinated linear
Using Tormach PCNC 1100 Series 3
7-2
32397 Rev C1-2
Programming language reference
motion, the motions can be coordinated so that acceleration and deceleration do not affect the
path.
If the rotational axes do not move, but the third linear axis does move, the trajectory of the
controlled point is a helix.
The feed rate during arc motion is as described in Feed Rate above. In the case of helical
motion, the rate is applied along the helix. Beware as other interpretations are used on other
systems.
7.1.9
Coolant
Flood coolant and mist coolant may each be turned on independently. They are turned off
together.
7.1.10 Dwell
A machining system may be commanded to dwell (i.e., keep all axes unmoving) for a specific
amount of time. The most common use of dwell is to break and clear chips or for a spindle to
get up to speed. The units in which you specify Dwell are either seconds or Milliseconds
depending on the setting on Configure>Logic.
7.1.11 Units
Units used for distances along the X-, Y- and Z-axes may be measured in millimeters or inches.
Units for all other quantities involved in machine control cannot be changed. Different
quantities use different specific units. Spindle speed is measured in revolutions per minute. The
positions of rotational axes are measured in degrees. Feed rates are expressed in current length
units per minute, or in degrees per minute, as described above.
Warning: We advise you to check very carefully the system’s response to changing units while
tool and fixture offsets are loaded into the tables, while these offsets are active and/or while a
part-program is executing
7.1.12 Current Position
The controlled point is always at some location called the “current position” and the Control
Software always knows where that is. The numbers representing the current position are
adjusted in the absence of any axis motion if any of several events take place:
•
Length units are changed (see Warning above);
•
Tool length offset is changed;
•
Coordinate system offsets are changed.
7.1.13 Selected Plane
There is always a “selected plane,” which must be the XY-plane, the YZ-plane or the XZ-plane
of the machining system. The Z-axis is, of course, perpendicular to the XY-plane, the X-axis to
the YZ-plane and the Y-axis to the XZ-plane.
7.1.14 Tool Table
Zero or one tool is assigned to each slot in the tool table.
7.1.15 Path Control Modes
The machining system may be put into any one of two path control modes: (1) exact stop mode,
(2) constant velocity mode. In exact stop mode, the machine stops briefly at the end of each
programmed move. In constant velocity mode, sharp corners of the path may be rounded
32397 Rev C1-2
7-3
Using Tormach PCNC 1100 Series 3
Programming language reference
slightly so that the feed rate may be kept up. These modes are to allow the user to control the
compromise involved in turning corners because a real machine has a finite acceleration due to
the inertia of its mechanism.
Exact stop does what it says. The machine will come to rest at each change of direction and the
tool will therefore precisely follow the commanded path.
Constant velocity will overlap acceleration in the new direction with deceleration in the current
one in order to keep the commanded feed rate. This implies a rounding of any corner but faster
and smoother cutting. This is particularly important in routing and plasma cutting. The lower
the acceleration of the machine axes, the greater will be the radius of the rounded corner.
In Plasma mode (set on Configure Logic dialog) the system attempts to optimize corner motion
for plasma cutting by a proprietary algorithm.
It is also possible to define a limiting angle so that changes in direction of more than this angle
will always be treated as Exact Stop even though Constant Velocity is selected. This allows
gentle corners to be smoother but avoids excessive rounding of sharp corners even on machines
with low acceleration on one or more axes. This feature is enabled in the Configure Logic
dialog and the limiting angle is set by a DRO. This setting will probably need to be chosen
experimentally depending on the characteristics of the machine tool and, perhaps, the toolpath
of an individual job.
7.2
Interpreter Interaction with Controls
7.2.1
Feed and Speed Override controls
The CS has commands which enable (M48) or disable (M49) the feed and speed override
switches. It is useful to be able to override these switches for some machining operations. The
idea is that optimal settings have been included in the program and the operator should not
change them.
7.2.2
Block Delete Control
If the block delete control is ON, lines of code which start with a slash (the block delete
character) are not executed. If the switch is off, such lines are executed.
7.2.3
Optional Program Stop Control
The optional program stop control works as follows. If this control is ON and an input line
contains an M01-code, program execution is stopped at the end on the commands on that line
until the Cycle Start button is pushed.
7.3
Tool File
The CS maintains a tool file for each of the 256 tools which can be used.
Each data line of the file contains the data for one tool. This allows the definition of the tool
length (Z-axis), tool diameter (for milling) and tool tip radius (for turning).
7.4
Part-programs Language
7.4.1
Overview
The language is based on lines of code. Each line (also called a “block”) may include
commands to the machining system to do several different things. Lines of code may be
collected in a file to make a program.
Using Tormach PCNC 1100 Series 3
7-4
32397 Rev C1-2
Programming language reference
A typical line of code consists of an optional line number at the beginning followed by one or
more “words.” A word consists of a letter followed by a number (or something that evaluates to
a number). A word may either give a command or provide an argument to a command. For
example, G1 X3 is a valid line of code with two words. “G1” is a command meaning “move in
a straight line at the programmed feed rate,” and “X3” provides an argument value (the value of
X should be 3 at the end of the move). Most commands start with either G (General) or M
(Miscellaneous). The words for these commands are called “G-codes” and “M-codes.”
The language has two commands (M2 or M30), either of which ends a program. A program
may end before the end of a file. Lines of a file that occur after the end of a program are not to
be executed in the normal flow so will generally be parts of subroutines.
7.4.2
Parameters
Note: There are significant differences between controls in the way parameters work. Do not
assume that code from another control will work in the same way with Mach 3. Tormach
advises that you avoid writing parametric G-code as this is difficult to debug and very difficult
for another operator to understand. Modern CAM virtually eliminates the need for it.
The CS maintains an array of 10,320 numerical parameters. Many of them have specific uses.
The parameters that are associated with fixtures are persistent over time. Other parameters will
be undefined when The CS is loaded. The parameters are preserved when the interpreter is
reset. Parameters 1 to 1000 can be used by the code of part-programs.
7.4.3
Coordinate Systems
The machining system has an absolute coordinate system and 254 work offset (fixture) systems.
You can set the offsets of tools by G10 L1 P~ X~ Z~. The “P word” defines the tool
number to be set.
You can set the offsets of the fixture systems using G10 L2 P~ X~ Y~ Z~ A~ B~ C~.
The P word defines the fixture to be set. The X, Y, Z, etc. words are the coordinates for the
origin of the axes in terms of the absolute coordinate system.
You can select one of the first seven work offsets by using G54, G55, G56, G57, G58 or G59.
Any of the 254 work offsets can be selected by G59 P~ (e.g., G59 P23 would select fixture
23). The absolute coordinate system can be selected by G59 P0.
You can offset the current coordinate system using G92 or G92.3. This offset will then be
applied on top of work offset coordinate systems. This offset may be cancelled with G92.1 or
G92.2.
You can make straight moves in the absolute machine coordinate system by using G53 with
either G0 or G1.
7.5
Formatting Code Lines (Block)
A permissible line of input code consists of the following, in order, with the restriction that
there is a maximum (currently 256) to the number of characters allowed on a line.
•
Optional block delete character, which is a slash "/"
•
Optional line number
•
Any number of words, parameter settings and comments
•
End of line marker (carriage return or line feed or both)
Any input not explicitly allowed is illegal and will cause the Interpreter to signal an error or to
ignore the line.
Currently programs are limited to 999,999 lines of code.
32397 Rev C1-2
7-5
Using Tormach PCNC 1100 Series 3
Programming language reference
Spaces and tabs are allowed anywhere on a line of code and do not change the meaning of the
line, except inside comments. This makes some strange-looking input legal. For example, the
Letter
A
B
C
D
F
G
H
I
J
K
L
M
N
O
P
Q
R
S
T
U
V
W
X
Y
Z
Meaning
A-axis of machine
B-axis of machine
C-axis of machine
tool radius compensation number
feed rate
general function (see Table 5)
tool length offset index
X-axis offset for arcs
X offset in G87 canned cycle
Y-axis offset for arcs
Y offset in G87 canned cycle
Z-axis offset for arcs
Z offset in G87 canned cycle
number of repetitions in canned
cycles/subroutines
key used with G10
miscellaneous function (see Table 7)
line number
Subroutine label number
dwell time in canned cycles
dwell time with G4
key used with G10
tapping depth in M871 – M874
feed increment in G83 canned cycle
repetitions of subroutine call
arc radius
canned cycle retract level
spindle speed
tool selection
Synonymous with A
Synonymous with B
Synonymous with C
X-axis of machine
Y-axis of machine
Z-axis of machine
Figure 7.1 – Word initial letters
line g0x +0. 12 34y 7 is equivalent to g0 x+0.1234 y7
Blank lines are allowed in the input. They will be ignored.
Input is case insensitive, except in comments; thus, any letter outside a comment may be in
upper or lower case without changing the meaning of a line.
Using Tormach PCNC 1100 Series 3
7-6
32397 Rev C1-2
Programming language reference
7.5.1
Line Number
A line number is the letter N followed by an integer (with no sign) between 0 and 99,999,999
written without commas. Line numbers may be repeated or used out of order, although normal
practice is to avoid such usage. A line number is not required to be used (and this omission is
common) but it must be in the proper place if it is used.
7.5.2
Subroutine Labels
A subroutine label is the letter O followed by an integer (with no sign) between 0 and 99999
written with no more than five digits (000009 is not permitted, for example). Subroutine labels
may be used in any order but must be unique in a program. Nothing else except a comment
should appear on the same line as a subroutine label. Note that line numbers are not permitted
with an O word in the current release of the software.
7.5.3
Word
A word is a letter other than N or O followed by a real value.
Words may begin with any of the letters (figure 7.1). The table includes N and O for
completeness, even though, as defined above, line numbers are not words. Several letters (I, J,
K, L, P and R) may have different meanings in different contexts.
A real value is some collection of characters that can be processed to come up with a number. A
real value may be an explicit number (such as 341 or -0.8807), a parameter value, an expression
or a unary operation value. Definitions of these follow immediately. Processing characters to
come up with a number is called “evaluating.” An explicit number evaluates to itself.
See warning above on risks of using parameters.
7.5.3.1
Number
The following rules are used for (explicit) numbers. In these rules a digit is a single character
between 0 and 9.
•
A number consists of (1) an optional plus or minus sign, followed by (2) zero to
many digits, followed, possibly, by (3) one decimal point, followed by (4) zero to
many digits – provided that there is at least one digit somewhere in the number.
•
There are two kinds of numbers: integers and decimals. An integer does not have a
decimal point in it; a decimal does.
•
Numbers may have any number of digits, subject to the limitation on line length.
Only about seventeen significant figures will be retained, however (enough for all
known applications).
•
A non-zero number with no sign as the first character is assumed to be positive.
Notice that initial (before the decimal point and the first non-zero digit) and trailing (after the
decimal point and the last non-zero digit) zeros are allowed but not required. A number written
with initial or trailing zeros will have the same value when it is read as if the extra zeros were
not there.
Numbers used for specific purposes by the Control Software are often restricted to some finite
set of values or some to some range of values. In many uses, decimal numbers must be close to
integers; this includes the values of indexes (for parameters and carousel slot numbers, for
example), M-codes and G-codes multiplied by ten. A decimal number which is supposed to be
close to an integer is considered close enough if it is within 0.0001 of an integer.
7.5.3.2
Parameter Value
A parameter value is the hash character # followed by a real value. The real value must evaluate
to an integer between 1 and 10320. The integer is the parameter identification number. Think of
32397 Rev C1-2
7-7
Using Tormach PCNC 1100 Series 3
Programming language reference
it as the number of a pigeon-hole and distinguish this from its real value which is whatever
number is stored in it.
The # character takes precedence over other operations, so that, for example, #1+2 means the
number found by adding 2 to the value of parameter 1, not the value found in parameter 3. Of
course, #[1+2] does mean the value found in parameter 3. The # character may be repeated;
for example ##2 means the value of the parameter whose index is the (integer) value of
parameter 2.
7.5.3.3
Expressions and Binary Operations
An expression is a set of characters starting with a left bracket ([) and ending with a balancing
right bracket (]). In between the brackets are numbers, parameter values, mathematical
operations and other expressions. An expression may be evaluated to produce a number. The
expressions on a line are evaluated when the line is read, before anything on the line is
executed. An example of an expression is:
[1+acos[0]-[#3**[4.0/2]]]
Binary operations appear only inside expressions. Nine binary operations are defined. There are
four basic mathematical operations: addition (+), subtraction (-), multiplication (*) and division
(/). There are three logical operations: non-exclusive or (OR), exclusive or (XOR) and logical
and (AND). The eighth operation is the modulus operation (MOD). The ninth operation is the
“power” operation (**) of raising the number on the left of the operation to the power on the
right.
The binary operations are divided into three groups. The first group is: power. The second
group is: multiplication, division and modulus. The third group is: addition, subtraction, logical
non-exclusive or, logical exclusive or and logical. If operations are strung together (for example
in the expression [2.0/3*1.5-5.5/11.0]), operations in the first group are to be
performed before operations in the second group and operations in the second group before
operations in the third group. If an expression contains more than one operation from the same
group (such as the first / and * in the example), the operation on the left is performed first.
Thus, the example is equivalent to: [((2.0/3)*1.5)-(5.5/11.0)] which simplifies to
[1.0-0.5] which is 0.5.
The logical operations and modulus are to be performed on any real numbers, not just on
integers. The number zero is equivalent to logical false and any non-zero number is equivalent
to logical true.
7.5.3.4
Unary Operation Value
A unary operation value is either “ATAN” followed by one expression divided by another
expression (for example ATAN[2]/[1+3]) or any other unary operation name followed by an
expression (for example SIN[90]). The unary operations are: ABS (absolute value), ACOS
(arc cosine), ASIN (arc sine), ATAN (arc tangent), COS (cosine), EXP (e raised to the given
power), FIX (round down), FUP (round up), LN (natural logarithm), ROUND (round to the
nearest whole number), SIN (sine), SQRT (square root) and TAN (tangent). Arguments to
unary operations which take angle measures (COS, SIN and TAN) are in degrees. Values
returned by unary operations which return angle measures (ACOS, ASIN and ATAN) are also
in degrees.
The FIX operation rounds towards the left (less positive or more negative) on a number line, so
that FIX[2.8]=2 and FIX[-2.8]=-3, for example. The FUP operation rounds towards the
right (more positive or less negative) on a number line; FUP[2.8]=3 and FUP[-2.8]=-2,
for example.
7.5.4
Parameter Setting
See warning above on risks of using parameters.
Using Tormach PCNC 1100 Series 3
7-8
32397 Rev C1-2
Programming language reference
A parameter setting is the following four items one after the other:
•
a pound character # ;
•
a real value which evaluates to an integer between 1 and 10320;
•
an equal sign = ;
•
a real value.
• For example “#3 = 15” is a parameter setting meaning “set parameter 3 to 15.”
A parameter setting does not take effect until after all parameter values on the same line have
been found. For example, if parameter 3 has been previously set to 15 and the line #3=6 G1
x#3 is interpreted, a straight move to a point where x equals 15 will occur and the value of
parameter 3 will be 6.
7.5.5
Comments and Messages
Printable characters and white space inside parentheses are considered a “comment.” A left
parenthesis always starts a comment. The comment ends at the first right parenthesis found
thereafter. Once a left parenthesis is placed on a line, a matching right parenthesis must appear
before the end of the line. Comments may not be nested; it is an error if a left parenthesis is
found after the start of a comment and before the end of the comment. Here is an example of a
line containing a comment: G80 M5 (stop motion)
Comments do not cause the machining system to do anything.
A comment contains a message if MSG, appears after the left parenthesis and before any other
printing characters. Variants of MSG, which include white space and lower case characters, are
allowed. Note the comma which is required. The rest of the characters before the right
parenthesis are considered to be a message to the operator. Messages are displayed on screen in
the “Error” intelligent label.
7.5.6
Item Repeats
A line may have any number of G words, but two G words from the same modal group may not
appear on the same line.
A line may have zero to four M words. Two M words from the same modal group may not
appear on the same line.
For all other legal letters, a line may have only one word beginning with that letter.
If a parameter setting of the same parameter is repeated on a line, #3=15 #3=6, for example,
only the last setting will take effect. It is silly, but not illegal, to set the same parameter twice on
the same line.
If more than one comment appears on a line, only the last one will be used; each of the other
comments will be read and its format will be checked, but it will be ignored thereafter. It is
expected that putting more than one comment on a line will be very rare.
7.5.7
Item Order
The three types of item whose order may vary on a line (as given at the beginning of this
section) are word, parameter setting and comment. Imagine that these three types of item are
divided into three groups by type.
The first group (the words) may be reordered in any way without changing the meaning of the
line.
If the second group (the parameter settings) is reordered, there will be no change in the meaning
of the line unless the same parameter is set more than once. In this case, only the last setting of
the parameter will take effect. For example, after the line #3=15 #3=6 has been interpreted,
32397 Rev C1-2
7-9
Using Tormach PCNC 1100 Series 3
Programming language reference
the value of parameter 3 will be 6. If the order is reversed to #3=6 #3=15 and the line is
interpreted, the value of parameter 3 will be 15.
If the third group (the comments) contains more than one comment and is reordered, only the
last comment will be used.
If each group is kept in order or reordered without changing the meaning of the line, then the
three groups may be interleaved in any way without changing the meaning of the line. For
example, the line g40 g01 #3=15 (so there!) #4=-7.0 has five items and means
exactly the same thing in any of the 120 possible orders – such as #4=-7.0 g01 #3=15
g40 (so there!) – for the five items.
7.5.8
Commands and Machine Modes
The Control Software has many commands that cause a machining system to change from one
mode to another. The mode stays active until some other command changes it implicitly or
explicitly. Such commands are called “modal.” For example, if coolant is turned on, it stays on
until it is explicitly turned off. The G-codes for motion are also modal. If a G1 (straight move)
command is given on one line, for example, it will be executed again on the next line if one or
more axis words is available on the line, unless an explicit command is given on that next line
using the axis words or canceling motion.
The modal groups for G-codes are
• group 1 = {G00, G01, G02, G03, G38.2, G80, G81, G82, G84, G85,
G86, G87, G88, G89} motion
• group 2 = {G17, G18, G19} plane selection
• group 3 = {G90, G91} distance mode
• group 5 = {G93, G94} feed rate mode
• group 6 = {G20, G21} units
• group 7 = {G40, G41, G42} cutter radius compensation
• group 8 = {G43, G49} tool length offset
• group 10 = {G98, G99} return mode in canned cycles
• group 12 = {G54, G55, G56, G57, G58, G59, G59.xxx} coordinate
system selection
• group 13 = {G61, G61.1, G64} path control mode
The modal groups for M-codes are:
♦ group 4 = {M0, M1, M2, M30} stopping
♦ group 6 = {M6} tool change
♦ group 7 = {M3, M4, M5} spindle turning
♦ group 8 = {M7, M8, M9} coolant (special case: M7 and M8 may be
active at the same time)
♦ group 9 = {M48, M49} enable/disable feed and speed override controls
In addition to the above modal groups, there is a group for non-modal
G-codes:
♦ group 0 = {G4, G10, G28, G30, G53, G92, G92.1, G92.2, G92.3}
Figure 7.2 – Modal groups
“Non-modal” codes have effect only on the lines on which they occur. For example, G4 (dwell)
is non-modal.
7.6
Modal Groups
Modal commands are arranged in sets called “modal groups,” and only one member of a modal
group may be in force at any given time. In general, a modal group contains commands for
Using Tormach PCNC 1100 Series 3
7-10
32397 Rev C1-2
Programming language reference
which it is logically impossible for two members to be in effect at the same time (e.g., measure
in inches vs. measure in millimeters). A machining system may be in many modes at the same
time, with one mode from each modal group being in effect (figure 7.2).
For several modal groups, when a machining system is ready to accept commands, one member
of the group must be in effect. There are default settings for these modal groups. When the
machining system is turned on or otherwise re-initialized, the default values are automatically
in effect.
Group 1, the first group on the table, is a group of G-codes for motion. One of these is always
in effect. That one is called the current motion mode.
It is an error to put a G-code from group 1 and a G-code from group 0 on the same line if both
of them use axis words. If an axis word-using G-code from group 1 is implicitly in effect on a
line (by having been activated on an earlier line) and a group 0 G-code that uses axis words
appears on the line, the activity of the group 1 G-code is suspended for that line. The axis wordusing G-codes from group 0 are G10, G28, G30 and G92.
The Control Software displays the current mode at the top of each screen.
7.7
G-codes
G-codes of the CS input language are shown in figure 7.3 and are described in more detail in
this section.
The descriptions contain command prototypes, set in courier type.
In the command prototypes, the tilde (~) stands for a real value. As described earlier, a real
value may be (1) an explicit number, 4.4, for example, (2) an expression, [2+2.4], for example,
(3) a parameter value, #88, for example or (4) a unary function value, acos[0], for example.
In most cases, if axis words (any or all of X~, Y~, Z~, A~, B~, C~, U~, V~, W~)
are given, they specify a destination point. Axis numbers relate to the currently active
coordinate system, unless explicitly described as being in the absolute coordinate system.
Where axis words are optional, any omitted axes will have their current value. Any items in the
command prototypes not explicitly described as optional are required. It is an error if a required
item is omitted.
U, V and W are synonyms for A, B and C. Use of A with U, B with V, etc. is erroneous (like
using A twice on a line). In the detailed descriptions of codes U, V and W are not explicitly
mentioned each time but are implied by A, B or C.
In the prototypes, the values following letters are often given as explicit numbers. Unless stated
otherwise, the explicit numbers can be real values. For example, G10 L2 could equally well be
written G[2*5] L[1+1]. If the value of parameter 100 were 2, G10 L#100 would also
mean the same. Using real values which are not explicit numbers as just shown in the examples
is rarely useful.
If L~ is written in a prototype the “~” will often be referred to as the “L number.” Similarly the
“~” in H~ may be called the “H number,” and so on for any other letter.
If a scale factor is applied to any axis then it will be applied to the value of the corresponding
X, Y, Z, A/U, B/V, C/W word and to the relevant I, J, K or R words when they are used.
32397 Rev C1-2
7-11
Using Tormach PCNC 1100 Series 3
Programming language reference
G00
G01
G02
G03
G04
G10
G12
G13
G15/G16
G17
G18
G19
G20/G21
G28
G28.1
G30
G31
G40
G41/G42
G43
G49
G50
G51
G52
G53
G54
G55
G56-58
G59
G61/G64
G68/G69
G73
G80
G81
G82
G83
G85
G86
G88
G89
G90
G91
G92
G92.x
G93
G94
G95
G98
G99
Summary of G-codes
Rapid positioning
Linear interpolation
Clockwise circular/helical interpolation
Counterclockwise circular/helical interpolation
Dwell
Coordinate system origin setting
Clockwise circular pocket
Counterclockwise circular pocket
Polar Coordinate moves in G00 and G01
XY Plane select
XZ plane select
YZ plane select
Inch/millimeter unit
Return home
Reference axes
Return home
Straight probe
Cancel cutter radius compensation
Start cutter radius compensation left/right
Apply tool length offset (plus)
Cancel tool length offset
Reset all scale factors to 1.0
Set axis data input scale factors
Temporary coordinate system offsets
Move in absolute machine coordinate system
Use fixture offset 1
Use fixture offset 2
Use fixture offset 3, 4, 5
Use fixture offset 6 / use general fixture number
Exact stop/Constant Velocity mode
Coordinate system rotation
Canned cycle - peck drilling
Cancel motion mode (including canned cycles)
Canned cycle – drilling
Canned cycle – drilling with dwell
Canned cycle – peck drilling
Canned cycle – boring, no dwell, feed out
Canned cycle – boring, spindle stop, rapid out
Canned cycle – boring, spindle stop, manual out
Canned cycle – boring, dwell, feed out
Absolute distance mode
Incremental distance mode
Offset coordinates and set parameters
Cancel G92 etc.
Inverse time feed mode
Feed per minute mode
Feed per rev mode
Initial level return after canned cycles
R-point level return after canned cycles
Figure 7.3 – Table of G-codes
Using Tormach PCNC 1100 Series 3
7-12
32397 Rev C1-2
Programming language reference
7.7.1
Rapid Linear Motion – G00
(a) For rapid linear motion, program: G0 X~ Y~ Z~ A~ where all the axis words are
optional, except that at least one must be used. The G00 is optional if the current motion mode
is G0. This will produce coordinated linear motion to the destination point at the current
traverse rate (or slower if the machine will not go that fast). It is expected that cutting will not
take place when a G00 command is executing.
(b) If G16 has been executed to set a Polar Origin then for rapid linear motion to a point
described by a radius and angle G0 X~ Y~ can be used. X~ is the radius of the line from the
G16 polar origin and Y~ is the angle in degrees measured with increasing values
counterclockwise from the 3 o’clock direction (i.e., the conventional four quadrant
conventions).
Coordinates of the current point at the time of executing the G16 are the polar origin.
It is an error if all axis words are omitted.
If cutter radius compensation is active, the motion will differ from the above; see Cutter
Compensation. If G53 is programmed on the same line, the motion will also differ; see
Absolute Coordinates.
Note that the G00 rapid move should have two
distinct movements to ensure that vertical
moves are always separate from horizontal
moves. In a typical rapid move toward the part,
the tool first rapids in the flat, horizontal XY
plane. Then, it feeds down in the Z axis. When
rapiding out of a part, the G00 command
always goes up in the Z axis first, then laterally
in the XY plane.
The G00 command is used to move the tool
quickly from one point to another without
cutting, thus allowing for quick tool
positioning.
Depending on where the tool is located, there are two
basic rules to follow for safety’s sake:
If the Z value represents a cutting move in the negative
direction, the X and Y axes should be executed first.
If the Z value represents a move in the positive
direction, the X and Y axes should be executed last.
Example:
7.7.2
N25 G00 X2.5 Y4.75
(Rapid to X2.5,Y4.75)
N30 Z0.1 (Rapid down to Z0.1)
Linear Motion at Feed Rate – G01
(a) For linear motion at feed rate (for cutting or not),
program: G01 X~ Y~ Z~ A~, where all the axis
words are optional, except that at least one must be
32397 Rev C1-2
7-13
As this diagram shows, if the basic
rules are not followed, an accident
can result. Improper use of G00
often occurs because clamps are
not taken into consideration.
Following the basic rules will
reduce any chance of error.
Using Tormach PCNC 1100 Series 3
Programming language reference
used. The G01 is optional if the current motion mode is G01. This will produce coordinated
linear motion to the destination point at the current feed rate (or slower if the machine will not
go that fast). (b) If G16 has been executed to set a polar origin then linear motion at feed rate to
a point described by a radius and angle G00 X~ Y~ can be used. X~ is the radius of the line
from the G16 polar origin and Y~ is the angle in degrees measured with increasing values
counterclockwise from the 3 o’clock direction (i.e., the conventional four quadrant
conventions).
Coordinates of the current point at the time of executing the G16 are the polar origin.
It is an error if all axis words are omitted.
If cutter radius compensation is active, the motion will differ from the above; see Cutter
Compensation. If G53 is programmed on the same line, the motion will also differ; see
Absolute Coordinates.
Linear Interpolation, or straightline feed
moves, on the flat XY plane (no Z values
are specified).
G01 command, using multi-axis
feed moves. All diagonal feed
moves are a result of a G01
command, where two or more axes
are used at once.
(Sample Program G01EX2:)
(Workpiece Size: X4, Y3, Z1)
(Tool: Tool #3, 3/8" Slot Drill)
(Tool Start Position: X0, Y0, Z1)
N2 G90 G80 G40 G54 G20 G17 G50 G94 G64 (safety block)
N5 G90 G20 (Block #5, absolute in inches)
N10 M06 T3 G43 H3 (Tool change to Tool #3)
N15 M03 S1250 (Spindle on CW at 1250 rpm)
N20 G00 X1.0 Y1.0 (Rapid over to X1,Y1)
N25 Z0.1 (Rapid down to Z0.1)
N30 G01 Z-0.125 F5 (Feed down to Z–0.125 at 5 ipm)
N35 X3 Y2 F10 (Feed diagonally to X3,Y2 at 10 ipm)
N40 G00 Z1.0 (Rapid up to Z1)
N45 X0.0 Y0.0 (Rapid over to X0,Y0)
N50 M05 (Spindle off)
N55 M30 (Program end)
In the sample program, several different examples of the G01 command are shown:
1. The first G01 command (in N30) instructs the machine to plunge feed the tool below the
surface of the part by 0.125 in. at a feedrate of 5 in./min.
2. N35 is a two-axis (X and Y) diagonal feed move, and the linear feedrate is increased to
10 ipm.
Note: Because there is contact between the cutting tool and the workpiece, it is imperative that
the proper spindle speeds and feedrates be used. It is the programmer’s responsibility to ensure
acceptable cutter speeds and feeds.
Using Tormach PCNC 1100 Series 3
7-14
32397 Rev C1-2
Programming language reference
7.7.3
Arc at Feed Rate – G02 and G03
A circular or helical arc is specified using either G02 (clockwise arc) or G03 (counterclockwise
arc). The axis of the circle or helix must be parallel to the X-, Y- or Z-axis of the machine
coordinate system. The axis (or, equivalently, the plane perpendicular to the axis) is selected
with G17 (Z-axis, XY-plane), G18 (Y-axis, XZ-plane) or G19 (X-axis, YZ-plane). If the arc is
circular, it lies in a plane parallel to the selected plane.
If a line of code makes an arc and includes
rotational axis motion, the rotational axes turn at
a constant rate so that the rotational motion starts
and finishes when the XYZ motion starts and
finishes. Lines of this sort are hardly ever
programmed.
If cutter radius compensation is active, the
motion will differ from the above; see Cutter
Compensation.
Two formats are allowed for specifying an arc.
We will call these the center format and the
radius format. In both formats the G02 or G03 is
optional if it is the current motion mode.
7.7.3.1
Radius Format Arc
In the radius format, the coordinates of the end
point of the arc in the selected plane are specified
along with the radius of the arc. Program: G02
X~ Y~ Z~ A~ R~ (or use G03 instead
of G02). R is the radius. The axis words
are all optional except that at least one of
the two words for the axes in the selected
plane must be used. The R number is the
radius. A positive radius indicates that the
arc turns through 180 degrees or less,
while a negative radius indicates a turn of
180 degrees to 359.999 degrees. If the arc
is helical, the value of the end point of
the arc on the coordinate axis parallel to
the axis of the helix is also specified.
Shows G02 arc start point, endpoint, and
center point.
It is an error if:
•
Both of the axis words for the
axes of the selected plane are
omitted;
•
No R word is given;
•
The end point of the arc is the same as the current point.
Shows G03 arc start point, endpoint, and center
point.
It is not good practice to program radius format arcs that are nearly full circles or are
semicircles (or nearly semicircles) because a small change in the location of the end point will
produce a much larger change in the location of the center of the circle (and, hence, the middle
of the arc). The magnification effect is large enough that rounding error in a number can
produce out-of-tolerance cuts. Nearly full circles are outrageously bad, semicircles (and nearly
so) are only very bad. Other size arcs (in the range tiny to 165 degrees or 195 to 345 degrees)
are OK.
Here is an example of a radius format command to mill an arc:
32397 Rev C1-2
7-15
Using Tormach PCNC 1100 Series 3
Programming language reference
G17 G02 X 1.0 Y 1.5 R 2.0 Z 0.5
That means to make a clockwise (as viewed from the positive Z-axis) circular or helical arc
whose axis is parallel to the Z-axis, ending where X=1.0, Y=1.5 and Z=0.5, with a radius of
2.0. If the starting value of Z is 0.5, this is an arc of a circle parallel to the XY-plane; otherwise
it is a helical arc.
7.7.3.2
Center Format Arc
In the center format, the coordinates of the end point of the arc in the selected plane are
specified along with the offsets of the center of the arc from the current location. In this format,
it is OK if the end point of the arc is the same as the current point.
It is an error if when the arc is projected on the selected plane, the distance from the current
point to the center differs from the distance from the end point to the center by more than
0.0002 inch (if inches are being used) or 0.002 millimeter (if millimeters are being used).
The center is specified using the I and J words. There are two ways of interpreting them. The
usual way is that I and J are the center relative to the current point at the start of the arc. This is
sometimes called Incremental IJ mode. The second way is that I and J specify the center as
actual coordinates in the current system. This is rather misleadingly called Absolute IJ mode.
The IJ mode is set using the button and LED on the Settings screen. The choice of modes is to
provide compatibility with commercial controllers. You will probably find Incremental to be
best. In Absolute it will, of course usually be necessary to use both I and J words unless by
chance the arc’s center is at the origin.
When the XY-plane is selected, program: G2 X~ Y~ Z~ A~ I~ J~ (or use G3 instead of
G2). The axis words are all optional except that at least one of X and Y must be used. I and J
are the offsets from the current location or coordinates – depending on IJ mode (X and Y
directions, respectively) of the center of the circle. I and J are optional except that at least one
of the two must be used. It is an error if:
•
X and Y are both omitted;
•
I and J are both omitted.
When the XZ-plane is selected, program: G02 X~ Y~ Z~ A~ I~ K~ (or use G03 instead
of G02). The axis words are all optional except that at least one of X and Z must be used. I and
K are the offsets from the current location or coordinates – depending on IJ mode (X and Z
directions, respectively) of the center of the circle. I and K are optional except that at least one
of the two must be used.
It is an error if:
•
X and Z are both omitted;
•
I and K are both omitted.
When the YZ-plane is selected, program: G02 X~ Y~ Z~ A~ J~ K~ (or use G03 instead
of G02). The axis words are all optional except that at least one of Y and Z must be used. J and
K are the offsets from the current location or coordinates – depending on IJ mode (Y and Z
directions, respectively) of the center of the circle. J and K are optional except that at least one
of the two must be used.
It is an error if:
•
Y and Z are both omitted;
•
J and K are both omitted.
Here is an example of a center format command to mill an arc in Incremental IJ mode:
G17 G02 X1.0 Y1.6 I0.3 J0.4 Z0.9
That means to make a clockwise (as viewed from the positive Z-axis) circular or helical arc
whose axis is parallel to the Z-axis, ending where X=1.0, Y=1.6 and Z=0.9, with its center
Using Tormach PCNC 1100 Series 3
7-16
32397 Rev C1-2
Programming language reference
offset in the X direction by 0.3 units from the current X location and offset in the Y direction by
0.4 units from the current Y location. If the current location has X=0.7, Y=0.7 at the outset, the
center will be at X=1.0, Y=1.1. If the starting value of Z is 0.9, this is a circular arc; otherwise it
is a helical arc. The radius of this arc would be 0.5.
The above arc in Absolute IJ mode would be:
G17 G02 X1.0 Y1.6 I1.0 J1.1 Z0.9
In the center format, the radius of the arc is not specified, but it may be found easily as the
distance from the center of the circle to either the current point or the end point of the arc.
(Sample Program G02EX3:)
(Workpiece Size: X4, Y3, Z1)
(Tool: Tool #2, 1/4" Slot Drill)
(Tool Start Position: X0, Y0, Z1)
N2 G90 G80 G40 G54 G20 G17 G50 G94 G64 (safety block)
N5 G90 G20
N10 M06 T2 G43 H2
N15 M03 S1200
N20 G00 X1 Y1
N25 Z0.1
N30 G01 Z-0.1 F5
N35 G02 X2 Y2 I1 J0 F20 (Arc feed CW, radius I1,J0 at 20 ipm)
N40 G01 X3.5
N45 G02 X3 Y0.5 R2 (Arc feed CW, radius 2)
N50 X1 Y1 R2 (Arc feed CW, radius 2)
N55 G00 Z0.1
N60 X2 Y1.5
N65 G01 Z-0.25
N70 G02 X2 Y1.5 I0.25 J-0.25 (Full circle arc feed move CW)
N75 G00 Z1
N80 X0 Y0
N85 M05
N90 M30
7.7.4
Dwell – G04
For a dwell, program: G04 P~. This will keep
the axes unmoving for the period of time in
seconds specified by the P number.
It is an error if the P number is negative.
(Sample Program G04EX5:)
(Workpiece Size: X3.5, Y2, Z0.5)
(Tool: Tool #1, 1/8" Slot Mill)
(Tool Start Position: X0, Y0, Z1)
The tool will pause for a short time only,
rarely more than several seconds. For a
definite program pause,
refer to the M00 and M01 commands.
Being nonmodal, the G04 must be
reentered each time Dwell is to be
executed.
N2 G90 G80 G40 G54 G20 G17 G50 G94 G64 (safety block)
N5 G90 G20 (Absolute programming in inch mode)
N10 M06 T1 G43 H1 (Tool change to Tool #1)
N15 M03 S1300 (Spindle on CW at 1300 rpm)
N20 G00 X3 Y1 Z0.1 (Rapid to X3,Y1,Z0.1)
N25 G01 Z-0.125 F5.0 (Feed down to Z–0.125 at 5 ipm)
N30 G04 P2 (Dwell for 2 seconds)
N35 G00 X2 Z0.1 (Rapid up to 0.1 and over to X2)
N40 G01 Z-0.125 F5.0 (Feed down to Z–0.125)
N45 G04 P1 (Dwell for 1 second)
N50 G00 Z1.0 (Rapid out to Z1)
N55 X0. Y0. (Rapid to X0, Y0)
N60 M05 (Spindle off )
N65 M30 (Program end)
32397 Rev C1-2
7-17
Using Tormach PCNC 1100 Series 3
Programming language reference
7.7.5
Coordinate System Data Tool and Work Offset Tables – G10
See details of tool and work offsets for further information on coordinate systems.
To set the offset values of a tool, program:
G10 L1 P~ X~ Z~ A~, where the P number must evaluate to an integer in the range 0 to
255 – the tool number – and offsets of the tool specified by the P number are reset to the given.
The A number will reset the tool tip radius. Only those values for which an axis word is
included on the line will be reset. The Tool diameter cannot be set in this way.
To set the coordinate values for the origin of a fixture coordinate system, program:
G10 L2 P~ X~ Y~ Z~ A~, where the P number must evaluate to an integer in the range 1
to 255 – the fixture number (Values 1 to 6 corresponding to G54 to G59) – and all axis words
are optional. The coordinates of the origin of the coordinate system specified by the P number
are reset to the coordinate values given (in terms of the absolute coordinate system). Only those
coordinates for which an axis word is included on the line will be reset.
It is an error if:
•
The P number does not evaluate to an integer in the range 0 to 255.
If origin offsets (made by G92 or G92.3) were in effect before G10 is used, they will continue
to be in effect afterwards.
The coordinate system whose origin is set by a G10 command may be active or inactive at the
time the G10 is executed.
The values set will not be persistent unless the tool or fixture tables are saved using the buttons
on Tables screen.
Example: G10 L2 P1 x3.5 y17.2 sets the origin of the first coordinate system (the one
selected by G54) to a point where X is 3.5 and Y is 17.2 (in absolute coordinates). The Z
coordinate of the origin (and the coordinates for any rotational axes) are whatever those
coordinates of the origin were before the line was executed.
7.7.6
Clockwise/Counterclockwise Circular Pocket – G12 and G13
These circular pocket commands are a sort of canned cycle which can be used to produce a
circular hole larger than the tool in use or with a suitable tool (like a woodruff key cutter) to cut
internal grooves for “O” rings etc.
Program: G12 I~ for a clockwise move and G13 I~ for a counterclockwise move.
The tool is moved in the X direction by the value of the I word and a circle cut in the direction
specified with the original X and Y coordinates as the center. The tool is returned to the center.
•
7.7.7
Its effect is undefined if the current plane is not XY
Exit and Enter Polar Mode – G15 and G16
It is possible for G0 and G1 moves in the X/Y plane only to specify coordinates as a radius and
angle relative to a temporary center point; program G16 to enter this mode. The current
coordinates of the controlled point are the temporary center.
Program: G15 to revert to normal Cartesian coordinates.
G0 X2.0 Y2.0
// normal G0 move to 2.0,2.0
G16 //start of polar mode.
G10 X1.0 Y45
( this will move to X = 2.7071, Y = 2.7071 which is a
spot on a circle) (of radius 1.0 at 45 degrees from
the initial coordinates of 2.0,2.0.)
Using Tormach PCNC 1100 Series 3
7-18
32397 Rev C1-2
Programming language reference
This can be very useful, for example, for drilling a circle of holes. The code below moves to a
circle of holes every 90 degrees on a circle of radius 2.5", center X = 0.5, Y = 0.6 and highspeed peck drills to Z = -0.6
G0 Z0.0
X0.5 Y0.6
(goto the center point)
G16
(enable Polar coordinates)
G81 X2.5 Y0.0 R0.0 Z-.6 F3
(in G16 mode the X becomes the offset from center and the Y
becomes the degrees of rotation from the center)
X2.5 Y90
X2.5 Y180
X2.6 Y270
G15
(cancels the g16)
G80
(cancels the canned cycle)
G0 Z0.0
X0.0 Y0.0
M30
Note:
(1) You must not make X or Y moves other than by using G0 or G1 when G16 is active;
(2) This G16 is different to a Fanuc implementation in that it uses the current point as the
polar center. The Fanuc version requires a lot of origin shifting to get the desired result for
any circle not centered on 0, 0.
7.7.8
Plane Selection – G17, G18 and G19
Program G17 to select the XY-plane, G18 to select the XZ-plane or G19 to select the YZ-plane.
A circular tool move in the G17
plane.
An example of an arc cut in
the G18 XZ plane. Keep in
mind that, because the
primary and secondary axes
are reversed, this arc is
actually a G03 command.
Tool cutting an arc in the
YZ plane – G19.
The effects of having a plane selected are discussed in under G2/3 and Canned cycles.
7.7.9
Length Units – G20 and G21
Program G20 to use inches for length units and program G21 to use millimeters.
It is usually a good idea to program either G20 or G21 near the beginning of a program before
any motion occurs and not to use either one anywhere else in the program. It is the
responsibility of the user to be sure all numbers are appropriate for use with the current length
units.
32397 Rev C1-2
7-19
Using Tormach PCNC 1100 Series 3
Programming language reference
7.7.10 Return to Home – G28 and G30
A home position is defined
To return to home position by way of the
programmed position, program:
G28 X~ Y~ Z~ A~ (or use G30). All axis
words are optional. The path is made by a traverse
move from the current position to the
programmed position, followed by a traverse
move to the home position. If no axis words are
programmed, the intermediate point is the current
point, only one move is made.
(Sample Program G28EX111:)
(Workpiece Size: X4, Y4, Z1)
(Tools: Tool #7, 1" Slot Drill)
(Tool #10, 1/2" HSS Drill)
(Tool Start Position: X0, Y0, Z1)
(Reference Point: X0, Y0, Z5 )
Cutter moves on the G28 command from
the start point to the intermediate point
and finally to the reference point.
N2 G90 G80 G40 G54 G20 G17 G50 G94 G64 (safety block)
N5 G90 G20
N10 M06 T7 G43 H7
N12 M03 S1000
N15 G00 X4.75 Y2
N17 Z0.1
N20 G01 Z-0.5 F5
N25 G01 X2 F10
N30 G00 Z0.25
N35 G28 X0 Y2.5 Z1 (Return to reference via X0,Y2.5,Z1)
N40 M06 T10 G43 H10
N45 M03 S2000
N50 G00 X2 Y2
N52 Z.5
N55 G01 Z-1.25 F5
N60 G00 Z1
N65 X0 Y0
N70 M05
N75 M30
7.7.11 Reference Axes – G28.1
Program: G28.1 X~ Y~ Z~ A~ to reference the given axes. The axes will move at the
current feed rate towards the home switch(es), as defined by the Configuration. When the
absolute machine coordinate reaches the value given by an axis word then the feed rate is set to
that defined by Configure>Config Referencing. Provided the current absolute position is
approximately correct, then this will give a soft stop onto the reference switch(es).
7.7.12 Straight Probe – G31
7.7.12.1 Straight Probe Command
Program: G31 X~ Y~ Z~ A~ to perform a straight probe operation. The probe will
conventionally be tool #99. The rotational axis words are allowed, but it is better to omit them.
If rotational axis words are used, the numbers must be the same as the current position numbers
Using Tormach PCNC 1100 Series 3
7-20
32397 Rev C1-2
Programming language reference
so that the rotational axes do not move. The linear axis words are optional, except that at least
one of them must be used. The tool in the spindle must be a probe.
It is an error if:
•
The current point is less than 0.01 inch (0.254 millimeter) from the programmed
point;
•
G31 is used in inverse time feed rate mode;
•
Any rotational axis is commanded to move;
•
No X-, Y- or Z-axis word is used.
In response to this command, the machine moves the controlled point (which should be at the
end of the probe tip) in a straight line at the current feed rate toward the programmed point; if
the probe trips, then the probe decelerates.
After successful probing, parameters 2000 to 2005 will be set to the coordinates of the location
of the controlled point at the time the probe tripped (not where it stopped) or if it does not trip
to the coordinates at the end of the move and a triplet giving X, Y and Z at the trip will be
written to the triplet file if it has been opened by the M40 macro/OpenDigFile() function
(q.v.). Code in macros or screen buttons can determine if a point is a trip or just the end of the
move by inspecting if the DIGITIZE input is active after the G31 command or comparing the
axis DROs with the requested move.
7.7.12.2 Using the Straight Probe Command
Using the straight probe command, if the probe shank is kept nominally parallel to the Z-axis
(i.e., any rotational axes are at zero) and the tool length offset for the probe is used, so that the
controlled point is at the end of the tip of the probe:
•
Without additional knowledge about the probe, the parallelism of a face of a part to the
XY-plane may, for example, be found;
•
If the probe tip radius is known approximately, the parallelism of a face of a part to the YZ
or XZ-plane may, for example, be found;
•
If the shank of the probe is known to be well-aligned with the Z-axis and the probe tip
radius is known approximately, the center of a circular hole, may, for example, be found;
•
If the shank of the probe is known to be well-aligned with the Z-axis and the probe tip
radius is known precisely, more uses may be made of the straight probe command, such as
finding the diameter of a circular hole.
If the straightness of the probe shank cannot be adjusted to high accuracy, it is desirable to
know the effective radii of the probe tip in at least the +X, -X, +Y and -Y directions. These
quantities can be stored in parameters either by being included in the parameter file or by being
set in a part-program.
Using the probe with rotational axes not set to zero is also feasible. Doing so is more complex
than when rotational axes are at zero and we do not deal with it here.
7.7.12.3 Example Code
As a usable example, see the code for finding the center and diameter of a circular hole. For this
code to yield accurate results, the probe shank must be well-aligned with the Z-axis, the cross
section of the probe tip at its widest point must be very circular and the probe tip radius (i.e.,
the radius of the circular cross section) must be known precisely. If the probe tip radius is
known only approximately (but the other conditions hold), the location of the hole center will
still be accurate, but the hole diameter will not.
N010 (probe to find center and diameter of circular hole)
N020 (This program will not run as given here. You have to)
N030 (insert numbers in place of <description of number>.)
32397 Rev C1-2
7-21
Using Tormach PCNC 1100 Series 3
Programming language reference
N040 (Delete lines N020, N030 and N040 when you do that.)
N050 G0 Z <Z-value of retracted position> F <feed rate>
N060 #1001=<nominal X-value of hole center>
N070 #1002=<nominal Y-value of hole center>
N080 #1003=<some Z-value inside the hole>
N090 #1004=<probe tip radius>
N100 #1005=[<nominal hole diameter>/2.0 - #1004]
N110 G0 X#1001 Y#1002 (move above nominal hole center)
N120 G0 Z#1003 (move into hole - to be cautious, substitute G1
for G0 here)
N130 G31 X[#1001 + #1005] (probe +X side of hole)
N140 #1011=#2000 (save results)
N150 G0 X#1001 Y#1002 (back to center of hole)
N160 G31 X[#1001 - #1005] (probe -X side of hole)
N170 #1021=[[#1011 + #2000] / 2.0] (find pretty good X-value of
hole center)
N180 G0 X#1021 Y#1002 (back to center of hole)
N190 G31 Y[#1002 + #1005] (probe +Y side of hole)
N200 #1012=#2001 (save results)
N210 G0 X#1021 Y#1002 (back to center of hole)
N220 G31 Y[#1002 - #1005] (probe -Y side of hole)
N230 #1022=[[#1012 + #2001] / 2.0] (find very good Y-value of
hole center)
N240 #1014=[#1012 - #2001 + [2 * #1004]] (find hole diameter in
Y-direction)
N250 G0 X#1021 Y#1022 (back to center of hole)
N260 G31 X[#1021 + #1005] (probe +X side of hole)
N270 #1031=#2000 (save results)
N280 G0 X#1021 Y#1022 (back to center of hole)
N290 G31 X[#1021 - #1005] (probe -X side of hole)
N300 #1041=[[#1031 + #2000] / 2.0] (find very good X-value of
hole center)
N310 #1024=[#1031 - #2000 + [2 * #1004]] (find hole diameter in
X-direction)
N320 #1034=[[#1014 + #1024] / 2.0] (find average hole diameter)
N330 #1035=[#1024 - #1014] (find difference in hole diameters)
N340 G0 X#1041 Y#1022 (back to center of hole)
N350 M2 (that’s all, folks)
In the above code, an entry of the form <description of a number> is meant to be replaced by an
actual number that matches the description of number. After this section of code has executed,
the X-value of the center will be in parameter 1041, the Y-value of the center in parameter 1022
and the diameter in parameter 1034. In addition, the diameter parallel to the X-axis will be in
parameter 1024, the diameter parallel to the Y-axis in parameter 1014 and the difference (an
indicator of circularity) in parameter 1035. The probe tip will be in the hole at the XY center of
the hole.
The example does not include a tool change to put a probe in the spindle. Add the tool change
code at the beginning, if needed.
7.7.13 Cutter Radius Compensation – G40, G41 and G42
Note: Cutter compensation is an area of active development for the Mach3 control software.
The current version of Mach3 implements a primitive version of cutter compensation (G41,
G42) which we do not recommend for most applications. The demonstration example in section
6.8 does work and G41, G42 can be used successfully under certain conditions, never the less,
there are enough exceptions to make programming with G41, G42 and exercise in frustration.
All modern CAM programs support path planning for tool offsets which offer a more practical
solution at this time
Using Tormach PCNC 1100 Series 3
7-22
32397 Rev C1-2
Programming language reference
To turn cutter radius compensation off, program: G40. It is OK to turn compensation off when
it is already off.
Cutter radius compensation may be performed only if the XY-plane is active.
To turn cutter radius compensation on left (i.e., the cutter stays to the left of the programmed
path when the tool radius is positive), program: G41 D~. To turn cutter radius compensation
on right (i.e., the cutter stays to the right of the programmed path when the tool radius is
positive), program: G42 D~. The D word is optional; if there is no D word, the radius of the
tool currently in the spindle will be used. If used, the D number should normally be the slot
number of the tool in the spindle, although this is not required. It is OK for the D number to be
zero; a radius value of zero will be used.
G41 and G42 can be qualified by a P-word. This will override the value of the diameter of the
tool (if any) given in the current tool table entry.
It is an error if:
•
The D number is not an integer, is negative or is larger than the number of carousel
slots;
•
The XY-plane is not active;
•
Cutter radius compensation is commanded to turn on when it is already on.
The behavior of the machining system when cutter radius compensation is ON is described in
the chapter on Cutter Compensation. Notice the importance of programming valid entry and
exit moves.
Note: The tool offsets must have been applied with a G43 H~ for compensation to work.
7.7.14 Tool Length Offsets – G43, G44 and G49
To use a tool length offset, program: G43 H~, where the H number is the desired index in the
tool table. It is expected that all entries in this table will be positive. The H number should be,
but does not have to be, the same as the slot number of the tool currently in the spindle. The H
number may be zero; an offset value of zero will be used. Omitting H has the same effect as a
zero value.
G44 is provided for compatibility and is used if entries in the table give negative offsets.
It is an error if the H number is not an integer, is negative or is larger than the number of
carousel slots.
To use no tool length offset, program: G49.
It is OK to program using the same offset already in use. It is also OK to program using no tool
length offset if none is currently being used.
It is strongly advised to put the G43 command on the same line (block) as the T~ and the M06
which actually implements the change. If this is done then the control software anticipates the
new offset during the time the operator has control for changing the tool. The operator can
change the work Z offset safely if this condition is met.
7.7.15 Scale Factors – G50 and G51
To define a scale factor which will be applied to an X, Y, Z, A, I & J word before it is used
program: G51 X~ Y~ Z~ A~ where the X, Y, Z etc. words are the scale factors for the
given axes. These values are, of course, never themselves scaled.
It is not permitted to use unequal scale factors to produce elliptical arcs with G2 or G3.
To reset the scale factors of all axes to 1.0 program: G50.
32397 Rev C1-2
7-23
Using Tormach PCNC 1100 Series 3
Programming language reference
7.7.16 Temporary Coordinate System Offset – G52
To offset the current point by a given positive or negative distance (without motion), program:
G52 X~ Y~ Z~ A~, where the axis words contain the offsets you want to provide. All axis
words are optional, except that at least one must be used. If an axis word is not used for a given
axis, the coordinate on that axis of the current point is not changed.
It is an error if all axis words are omitted.
G52 and G92 use common internal mechanisms in the CS and may not be used together.
When G52 is executed, the origin of the currently active coordinate system moves by the values
given.
The effect of G52 is cancelled by programming: G52 X0 Y0 etc.
Here is an example. Suppose the current point is at X=4 in the currently specified coordinate
system, then G52 X7 sets the X-axis offset to 7 and so causes the X-coordinate of the current
point to be -3.
The axis offsets are always used when motion is specified in absolute distance mode using any
of the fixture coordinate systems. Thus all fixture coordinate systems are affected by G52.
7.7.17 Move in Absolute Coordinates – G53
For linear motion to a point expressed in absolute coordinates, program: G1 G53 X~ Y~ Z~
A~ (or similarly with G0 instead of G1), where all the axis words are optional, except that at
least one must be used. The G0 or G1 is optional if it is in the current motion mode. G53 is not
modal and must be programmed on each line on which it is intended to be active. This will
produce coordinated linear motion to the programmed point. If G1 is active, the speed of
motion is the current feed rate (or slower if the machine will not go that fast). If G0 is active,
the speed of motion is the current traverse rate (or slower if the machine will not go that fast).
It is an error if:
•
G53 is used without G0 or G1 being active;
• G53 is used while cutter radius compensation is on.
See relevant chapter for an overview of coordinate systems.
7.7.18 Select Work Offset Coordinate System – G54 to G59 & G59 P~
To select work offset #1, program: G54 and similarly for the first six offsets. The systemnumber-G-code pairs are: (1-G54), (2-G55), (3-G56), (4-G57), (5-G58), (6-G59).
To access any of the 254 work offsets (1 - 254) program: G59 P~ where the P word gives the
required offset number. Thus G59 P5 is identical in effect to G58.
It is an error if one of these G-codes is used while cutter radius compensation is on.
See relevant chapter for an overview of coordinate systems.
(Sample Program G54EX19:)
(Workpiece Size: X8, Y5, Z2)
(Tool: Tool #6, 3/4" HSS Drill)
(Tool Start Position: X0, Y0, Z1)
(Workpiece Coordinate system 2: X1, Y1, Z0)
(Workpiece Coordinate system 3: X5, Y1, Z0)
N2 G90 G80 G40 G54 G20 G17 G50 G94 G64 (safety block)
N5 G90 G80 G20
N10 M06 T6 G43 H6
N15 M03 S1300
N20 G55 G00 X1.0 Y1.0 (Rapid to X1, Y1 of work coordinate system 2)
N25 Z0.5
Using Tormach PCNC 1100 Series 3
7-24
32397 Rev C1-2
Programming language reference
N30 G82 Z-0.25 R0.125 P1 F5
N35 Y2
N40 X2
N45 Y1
N50 X1.5 Y1.5
N60 G80 G00 Z1
N65 G56 G00 X1.0 Y1.0 (Rapid to X1, Y1 of work coordinate system 3)
N70 Z0.5
N75 G82 Z-0.25 R0.125 P1 F5
N80 Y2
N85 X2
N90 Y1
N95 X1.5 Y1.5
N100 G80 G00 Z1
N105 X0 Y0
N110 M05
N115 M30
7.7.19 Set Path Control Mode – G61 and G64
Program: G61 to put the machining system into exact stop mode or G64 for constant velocity
mode. It is OK to program for the mode that is already active. These modes are described in
detail in 7.1.15 above.
7.7.20 Coordinate system rotation – G68 and G69
A rotation transformation can be applied to the controlled point coordinates commanded by a
part program or by the MDI line. To do this program G68 X~ Y~ R~ The X and Y words
specify the center about which the rotation is to be applied in the current coordinate system. R
is the angle of rotation in degrees with positive values being counter-clockwise.
If X or Y are omitted then zero is assumed. A and B can be used as synonyms for X and Y
respectively.
To cancel rotation program G69. If a G68 is used while rotation is in operation a G69 is implied
before it. In other words successive G68s are not cumulative and the X and Y points are always
in an un-rotated system.
When a rotation is in use the X and Y axis DROs will be red to remind the operator that these
values are program coordinate values which will be rotated.
This function can be used to compensate for work not exactly aligned on the table, to rotate the
operation of a part program if it is coded with Y travel greater than X and so the work will not
fit on the table or as software "vise soft-jaws".
Note:
•
G68 may only be used in the XY plane (G17 mode)
•
The effects of changing work offsets when a rotation transformation is in effect will be
non-intuitive so it is wiser not to program this. Indeed care should be taken proving any
program including transformations.
•
There is very little standardization of the functions of this code across different CNC
controls so careful checks should be made on code written for other machines.
•
Jogging always takes place in the direction of the machine axes. The toolpath display
frame is oriented to the physical axes and will show the part at the angle at which it will
be cut.
32397 Rev C1-2
7-25
Using Tormach PCNC 1100 Series 3
Programming language reference
7.7.21 Canned Cycle – High Speed Peck Drill – G73
The G73 cycle is intended for deep drilling or milling with chip breaking. See also G83. The
retracts in this cycle break the chip but do not totally retract the drill from the hole. It is suitable
for tools with long flutes which will clear the broken chips from the hole. This cycle takes a Q
number which represents a “delta” increment along the Z-axis. Program:
G73 X~ Y~ Z~ A~ R~ L~ Q~
•
Preliminary motion, as described in G81 to 89 canned cycles.
•
Move the Z-axis only at the current feed rate downward by delta or to the Z position,
whichever is less deep.
•
Rapid back out by the distance defined in the G73 Pullback DRO on the Settings screen.
•
Rapid back down to the bottom of the current hole, but backed off a bit.
•
Repeat steps 1, 2 and 3 until the Z position is reached at step 1.
• Retract the Z-axis at traverse rate to clear Z.
It is an error if the Q number is negative or zero.
The following sample program demonstrates the G73 command.
(Sample Program G73EX20:)
(Workpiece Size: X4, Y3, Z1)
(Tool: Tool #3, 3/8" HSS Drill)
(Tool Start Position: X0, Y0, Z1)
N2 G90 G80 G40
N5 G90 G80 G20
N10 M06 T3 G43
N15 M03 S1200
N20 G00 X1 Y1
N25 G73 Z-0.75
N30 X2.0
N35 X3.0
N40 Y2.0
N45 X2.0
N50 X1.0
N55 G80 G00 Z1
N60 X0 Y0
N65 M05
N70 M30
G54 G20 G17 G50 G94 G64 (safety block)
H3
R0.125 Q0.0625 F5 (Invoke G73 cycle)
(Canned cycle cancel)
7.7.22 Cancel Modal Motion – G80
Program: G80 to ensure no axis motion will occur, to terminate canned cycles etc. Note that it
cancels the current G2 or G3 mode so this must be re-established for the next move that is
required. This particularly affects people adapting a CAM postprocessors from another machine
as this behavior varies between different CNC controls.
It is an error if:
•
Axis words are programmed when G80 is active, unless a modal group 0 G-code is
programmed which uses axis words.
7.7.23 Canned Cycles – G81 to G89
The canned cycles G81 through G89 have been implemented as described in this section. Two
examples are given with the description of G81 below.
All canned cycles are performed with respect to the currently selected plane. Any of the three
planes (XY, YZ, and ZX) may be selected. Throughout this section, most of the descriptions
Using Tormach PCNC 1100 Series 3
7-26
32397 Rev C1-2
Programming language reference
assume the XY-plane has been selected. The behavior is always analogous if the YZ or XZplane is selected.
Rotational axis words are allowed in canned cycles, but it is better to omit them. If rotational
axis words are used, the numbers must be the same as the current position numbers so that the
rotational axes do not move.
All canned cycles use X, Y, R and Z numbers in the NC-code. These numbers are used to
determine X, Y, R and Z positions. The R (usually meaning retract) position is along the axis
perpendicular to the currently selected plane (Z-axis for XY-plane, X-axis for YZ-plane, Y-axis
for XZ-plane). Some canned cycles use additional arguments.
For canned cycles, we will call a number “sticky” if, when the same cycle is used on several
lines of code in a row, the number must be used the first time, but is optional on the rest of the
lines. Sticky numbers keep their value on the rest of the lines if they are not explicitly
programmed to be different. The R number is always sticky.
In incremental distance mode: when the XY-plane is selected, X, Y and R numbers are treated
as increments to the current position and Z as an increment from the Z-axis position before the
move involving Z takes place; when the YZ or XZ-plane is selected, treatment of the axis
words is analogous. In absolute distance mode, the X, Y, R and Z numbers are absolute
positions in the current coordinate system.
The L number is optional and represents the number of repeats. L=0 is not allowed. If the repeat
feature is used, it is normally used in incremental distance mode, so that the same sequence of
motions is repeated in several equally spaced places along a straight line. In absolute distance
mode, L > 1 means “do the same cycle in the same place several times,” Omitting the L word is
equivalent to specifying L=1. The L number is not sticky.
When L>1 in incremental mode with the XY-plane selected, the X and Y positions are
determined by adding the given X and Y numbers either to the current X and Y positions (on
the first go-around) or to the X and Y positions at the end of the previous go-around (on the
repetitions). The R and Z positions do not change during the repeats.
The height of the retract move at the end of each repeat (called “clear Z” in the descriptions
below) is determined by the setting of the retract mode: either to the original Z position (if that
is above the R position and the retract mode is G98) or otherwise to the R position.
It is an error if:
•
X, Y and Z words are all missing during a canned cycle;
•
A P number is required and a negative P number is used;
•
An L number is used that does not evaluate to a positive integer;
•
Rotational axis motion is used during a canned cycle;
•
Inverse time feed rate is active during a canned cycle;
•
Cutter radius compensation is active during a canned cycle.
When the XY plane is active, the Z number is sticky and it is an error if:
•
The Z number is missing and the same canned cycle was not already active;
•
The R number is less than the Z number.
When the XZ plane is active, the Y number is sticky and it is an error if:
•
The Y number is missing and the same canned cycle was not already active;
•
The R number is less than the Y number.
When the YZ plane is active, the X number is sticky and it is an error if:
32397 Rev C1-2
•
The X number is missing and the same canned cycle was not already active;
•
The R number is less than the X number.
7-27
Using Tormach PCNC 1100 Series 3
Programming language reference
7.7.23.1 Preliminary and In-Between Motion
At the very beginning of the execution of any of the canned cycles, with the XY-plane selected,
if the current Z position is below the R position, the Z-axis is traversed to the R position. This
happens only once, regardless of the value of L.
In addition, at the beginning of the first cycle and each repeat, the following one or two moves
are made:
• A straight traverse parallel to the XY-plane to the given XY-position;
• A straight traverse of the Z-axis only to the R position, if it is not already at the R
position.
If the XZ or YZ plane is active, the preliminary and in-between motions are analogous.
7.7.23.2 G81 Cycle
The G81 cycle is intended for drilling. Program: G81 X~ Y~ Z~ A~ R~ L~
•
Preliminary motion, as described above.
•
Move the Z-axis only at the current feed rate to the Z position.
•
Retract the Z-axis at traverse rate to clear Z.
Example 1: Suppose the current position is (1, 2, 3) and the XY-plane has been selected and
the following line of NC-code is interpreted.
G90 G81 G98 X4 Y5 Z1.5 R2.8
This calls for absolute distance mode (G90), old “Z” retract mode (G98) and calls for the G81
drilling cycle to be performed once. The X number and X position are 4. The Y number and Y
position are 5. The Z number and Z position are 1.5. The R number and clear Z are 2.8. The
following moves take place.
• a traverse parallel to the XY-plane to (4,5,3);
• a traverse parallel to the Z-axis to (4,5,2.8);
• a feed parallel to the Z-axis to (4,5,1.5);
• a traverse parallel to the Z-axis to (4,5,3).
Example 2: Suppose the current position is (1, 2, 3) and the XY-plane has been selected and
the following line of NC-code is interpreted.
G91 G81 G98 X4 Y5 Z-0.6 R1.8 L3
This calls for incremental distance mode (G91), old “Z” retract mode and calls for the G81
drilling cycle to be repeated three times. The X number is 4, the Y number is 5, the Z number is
-0.6 and the R number is 1.8. The initial X position is 5 (=1+4), the initial Y position is 7
(=2+5), the clear Z position is 4.8 (=1.8+3) and the Z position is 4.2 (=4.8-0.6). Old Z is 3.0
The first move is a traverse along the Z-axis to (1,2,4.8), since old Z < clear Z.
The first repeat consists of 3 moves.
• a traverse parallel to the XY-plane to (5,7,4.8);
• a feed parallel to the Z-axis to (5,7, 4.2);
• a traverse parallel to the Z-axis to (5,7,4.8).
The second repeat consists of 3 moves. The X position is reset to 9 (=5+4) and the Y position to
12 (=7+5).
• a traverse parallel to the XY-plane to (9,12,4.8);
• a feed parallel to the Z-axis to (9,12, 4.2);
• a traverse parallel to the Z-axis to (9,12,4.8).
Using Tormach PCNC 1100 Series 3
7-28
32397 Rev C1-2
Programming language reference
The third repeat consists of 3 moves. The X position is reset to 13 (=9+4) and the Y position to
17 (=12+5).
• a traverse parallel to the XY-plane to (13,17,4.8);
• a feed parallel to the Z-axis to (13,17, 4.2);
• a traverse parallel to the Z-axis to (13,17,4.8).
Execute the following to observe the G81 drill cycle. Remember, the G81 command follows a
certain sequence.
(Sample Program G81EX18:)
(Workpiece Size: X4, Y3, Z1)
(Tool: Tool #6, 3/4" HSS Drill)
(Tool Start Position: X0, Y0, Z1)
N2 G90 G80 G40
N5 G90 G80 G20
N10 M06 T6 G43
N15 M03 S1300
N20 G00 X1 Y1
N25 Z0.5
N30 G81 Z-0.25
N35 X2
N40 X3
N45 Y2
N50 X2
N55 X1
N60 G80 G00 Z1
N65 X0 Y0
N70 M05
N75 M30
G54 G20 G17 G50 G94 G64 (safety block)
H6
R0.125 F5 (Drill cycle invoked)
(Cancel canned cycles)
7.7.23.3 G82 Cycle
The G82 cycle is intended for drilling. Program:
G82 X~ Y~ Z~ A~ R~ L~ P~
•
Preliminary motion, as described above.
•
Move the Z-axis only at the current feed rate to the Z position.
•
Dwell for the P number of seconds.
•
Retract the Z-axis at traverse rate to clear Z.
7.7.23.4 G83 Cycle
The G83 cycle (often called peck drilling) is intended for deep drilling or milling with chip
breaking. See also G73. The retracts in this cycle clear the hole of chips and cut off any long
stringers (which are common when drilling in aluminum). This cycle takes a Q number which
represents a “delta” increment along the Z-axis. Program:
G83 X~ Y~ Z~ A~ R~ L~ Q~
•
Preliminary motion, as described above.
•
Move the Z-axis only at the current feed rate downward by delta or to the Z position,
whichever is less deep.
•
Rapid back out to the clear Z.
•
Rapid back down to the current hole bottom, backed off a bit.
•
Repeat steps 1, 2 and 3 until the Z position is reached at step 1.
32397 Rev C1-2
7-29
Using Tormach PCNC 1100 Series 3
Programming language reference
•
Retract the Z-axis at traverse rate to clear Z.
It is an error if:
•
The Q number is negative or zero.
7.7.23.5 G85 Cycle
The G85 cycle is intended for boring or reaming, but could be used for drilling or milling.
Program: G85 X~ Y~ Z~ A~ R~ L~
•
Preliminary motion, as described above.
•
Move the Z-axis only at the current feed rate to the Z position.
•
Retract the Z-axis at the current feed rate to clear Z.
7.7.23.6 G86 Cycle
The G86 cycle is intended for boring. This cycle uses a P number for the number of seconds to
dwell. Program: G86 X~ Y~ Z~ A~ R~ L~ P~
•
Preliminary motion, as described above.
•
Move the Z-axis only at the current feed rate to the Z position.
•
Dwell for the P number of seconds.
•
Stop the spindle turning.
•
Retract the Z-axis at traverse rate to clear Z.
•
Restart the spindle in the direction it was going.
The spindle must be turning before this cycle is used. It is an error if:
•
The spindle is not turning before this cycle is executed.
7.7.23.7 G88 Cycle
The G88 cycle is intended for boring. This cycle uses a P word, where P specifies the number
of seconds to dwell. Program: G88 X~ Y~ Z~ A~ R~ L~ P~
7.7.23.8
•
Preliminary motion, as described above.
•
Move the Z-axis only at the current feed rate to the Z position.
•
Dwell for the P number of seconds.
•
Stop the spindle turning.
•
Stop the program so the operator can retract the spindle manually.
•
Restart the spindle in the direction it was going.
G89 Cycle
The G89 cycle is intended for boring. This cycle uses a P number, where P specifies the number
of seconds to dwell. Program: G89 X~ Y~ Z~ A~ R~ L~ P~
•
Preliminary motion, as described above.
•
Move the Z-axis only at the current feed rate to the Z position.
•
Dwell for the P number of seconds.
•
Retract the Z-axis at the current feed rate to clear Z.
7.7.24 Distance Mode – G90 and G91
Interpretation of the CS-code can be in one of two distance modes: absolute or incremental.
Using Tormach PCNC 1100 Series 3
7-30
32397 Rev C1-2
Programming language reference
To go into absolute distance mode, program: G90. In absolute distance mode, axis numbers (X,
Y, Z, A) usually represent positions in terms of the currently active coordinate system. Any
exceptions to that rule are described explicitly in this section describing G-codes.
To go into incremental distance mode, program: G91. In incremental distance mode, axis
numbers (X, Y, Z, A) usually represent increments from the current values of the numbers.
I and J numbers always represent increments, regardless of the distance mode setting. K
numbers represent increments.
7.7.25 G92 Offsets – G92, G92.1, G92.2 and G92.3
See the chapter on coordinate systems for full details. You are strongly advised not to use this
legacy feature on any axis where there is another offset applied.
To make the current point have the coordinates you want (without motion), program:
G92 X~ Y~ Z~ A~, where the axis words contain the axis numbers you want. All axis
words are optional, except that at least one must be used. If an axis word is not used for a given
axis, the coordinate on that axis of the current point is not changed.
It is an error if all axis words are omitted.
G52 and G92 use common internal mechanisms in the CS and may not be used together.
When G92 is executed, the origin of the currently active coordinate system moves. To do this,
origin offsets are calculated so that the coordinates of the current point with respect to the
moved origin are as specified on the line containing the G92. In addition, parameters 5211 to
5214 are set to the X-, Y-, Z-, A-axis offsets. The offset for an axis is the amount the origin
must be moved so that the coordinate of the controlled point on the axis has the specified value.
Here is an example. Suppose the current point is at X=4 in the currently specified coordinate
system and the current X-axis offset is zero, then G92 X7 sets the X-axis offset to -3, sets
parameter 5211 to -3 and causes the X-coordinate of the current point to be 7.
The axis offsets are always used when motion is specified in absolute distance mode using any
of the fixture coordinate systems. Thus, all fixture coordinate systems are affected by G92.
Being in incremental distance mode has no effect on the action of G92.
Non-zero offsets may already be in effect when the G92 is called. They are in effect discarded
before the new value is applied. Mathematically the new value of each offset is A+B, where A
is what the offset would be if the old offset were zero and B is the old offset. For example, after
the previous example, the X-value of the current point is 7. If G92 X9 is then programmed, the
new X-axis offset is -5, which is calculated by [[7-9] + -3]. Put another way the G92 X9
produces the same offset whatever G92 offset was already in place.
To reset axis offsets to zero, program: G92.1 or G92.2 G92.1 sets parameters 5211 to 5214 to
zero, whereas G92.2 leaves their current values alone.
To set the axis offset values to the values given in parameters 5211 to 5214, program: G92.3
You can set axis offsets in one program and use the same offsets in another program by
programming G92 in the first program. This will set parameters 5211 to 5214. Do not use
G92.1 in the remainder of the first program. The parameter values will be saved when the first
program exits and restored when the second one starts up. Use G92.3 near the beginning of the
second program. That will restore the offsets saved in the first program.
7.7.26 Feed Rate Mode – G93, G94 and G95
Three feed rate modes are recognized: inverse time, units per minute and units per revolution of
spindle. Program: G93 to start the inverse time mode (this is very infrequently employed).
Program: G94 to start the units per minute mode. Program: G95 to start the units per rev mode.
32397 Rev C1-2
7-31
Using Tormach PCNC 1100 Series 3
Programming language reference
In inverse time feed rate mode, an F word means the move should be completed in [one divided
by the F number] minutes. For example, if the F number is 2.0, the move should be completed
in half a minute.
In units per minute feed rate mode, an F word on the line is interpreted to mean the controlled
point should move at a certain number of inches per minute, millimeters per minute or degrees
per minute, depending upon what length units are being used and which axis or axes are
moving.
In units per rev feed rate mode, an F word on the line is interpreted to mean the controlled point
should move at a certain number of inches per spindle revolution, millimeters per spindle
revolution or degrees per spindle revolution, depending upon what length units are being used
and which axis or axes are moving.
When the inverse time feed rate mode is active, an F word must appear on every line which has
a G1, G2 or G3 motion and an F word on a line that does not have G1, G2 or G3 is ignored.
Being in inverse time feed rate mode does not affect G0 (rapid traverse) motions.
It is an error if inverse time feed rate mode is active and a line with G1, G2 or G3 (explicitly or
implicitly) does not have an F word.
7.7.27 Canned Cycle Return Level – G98 and G99
When the spindle retracts during canned cycles, there is a choice of how far it retracts:
1. Retract perpendicular to the selected plane to the position indicated by the R word;
2. Retract perpendicular to the selected plane to the position that axis was in just before the
canned cycle started (unless that position is lower than the position indicated by the R
word, in which case use the R word position).
To use option 1, program: G99. To use option 2, program: G98. Remember that the R word
has different meanings in absolute distance mode and incremental distance mode.
7.8
Built-in M-codes
M-codes interpreted directly by the CS are shown in figure 7.5.
7.8.1
Program Stopping and Ending – M0, M1, M2 and M30
To stop a running program temporarily (regardless of the setting of the optional stop switch),
program: M0.
To stop a running program temporarily (but only if the optional stop switch is on), program:
M1.
It is OK to program M0 and M1 in MDI mode, but the effect will probably not be noticeable,
because normal behavior in MDI mode is to stop after each line of input, anyway.
If a program is stopped by an M0, M1, pressing the cycle start button will restart the program at
the following line.
To end a program, program: M2 or M30. M2 leaves the next line to be executed as the M2 line.
M30 “rewinds” the G-code file. These commands can have the following effects depending on
the options chosen on the Configure>Logic dialog:
•
Axis offsets are set to zero (like G92.2) and origin offsets are set to the default (like
G54).
•
Selected plane is set to XY (like G17).
•
Distance mode is set to absolute (like G90).
•
Feed rate mode is set to Units per minute mode (like G94).
Using Tormach PCNC 1100 Series 3
7-32
32397 Rev C1-2
Programming language reference
•
Feed and speed overrides are set to ON (like M48).
•
Cutter compensation is turned off (like G40).
•
The spindle is stopped (like M5).
•
The current motion mode is set to G1 (like G1).
•
Coolant is turned off (like M9).
No more lines of code in the file will be executed after the M2 or M30 command is executed.
Pressing cycle start will resume the program (M2) or start the program back at the beginning of
the file (M30).
7.8.2
Spindle Control – M3, M4 and M5
To start the spindle turning clockwise at the currently programmed speed, program: M3.
To start the spindle turning counterclockwise at the currently programmed speed, program: M4.
For a PWM or Step/Dir spindle the speed is programmed by the S word. For an on/off spindle
control it will be set by the gearing/pulleys on the machine.
To stop the spindle from turning, program: M5.
It is OK to use M3 or M4 if the spindle speed is set to zero; if this is done (or if the speed
M-code
M0
M1
M2
M3/4
M5
M6
M7
M8
M9
M30
M47
M48
M49
M98
M99
M871, M872, M873, M8741
M9981
Meaning
Program stop
Optional program stop
Program end
Rotate spindle clockwise/counterclockwise
Stop spindle rotation
Tool change (by two macros)
Mist coolant on
Flood coolant on
All coolant off
Program end and Rewind
Repeat program from first line
Enable speed and feed override
Disable speed and feed override
Call subroutine
Return from subroutine/repeat
Tapping Cycles
Move to tool change position
Figure 7.4 – Built in M-codes
Note 1: These codes are “built in," but application specific to the PCNC 1100
override switch is enabled and set to zero), the spindle will not start turning. If, later, the spindle
speed is set above zero (or the override switch is turned up), the spindle will start turning. It is
permitted to use M3 or M4 when the spindle is already turning or to use M5 when the spindle is
already stopped but see the discussion on safety interlocks in configuration for the implications
of a sequence that would reverse an already running spindle.
7.8.3
Tool change – M6
Provided tool change requests are not to be ignored (as defined in Configure>Logic), The CS
will call a macro (q.v.) M6Start when the command is encountered. It will then wait for Cycle
32397 Rev C1-2
7-33
Using Tormach PCNC 1100 Series 3
Programming language reference
Start to be pressed, execute the macro M6End and continue running the part-program. You can
provide Visual Basic code in the macros to operate your own mechanical tool changer and to
move the axes to a convenient location for tool changing if you wish.
You are strongly advised to put the T~, the M06 and the G43 H~ on one line (block) of code.
See G43 for more details.
7.8.4
Coolant Control – M7, M8 and M9
To turn mist coolant on, program: M7.
To turn flood coolant on, program: M8.
To turn all coolant off, program: M9.
It is always OK to use any of these commands, regardless of what coolant is on or off.
7.8.5
Re-run from First Line – M47
On encountering an M47 the part-program will continue running from its first line.
It is an error if M47 is executed in a subroutine.
The run can be stopped by the Pause or Stop buttons.
See also the use of M99 outside a subroutine to achieve the same effect.
7.8.6
Override Control – M48 and M49
To enable the speed and feed override, program: M48. To disable both overrides, program:
M49. It is OK to enable or disable the switches when they are already enabled or disabled.
7.8.7
Call Subroutine – M98
To call a subroutine program: M98 P~ L~ or M98 ~P ~Q. The program must contain a
letter O line with the number of the P word of the Call (for instance O1, O125, O777). This O
line is a sort of “label” which indicates the start of the subroutine. The O line may not have a
line number (e.g N123 O777) on it. The O line and the following code, will normally be written
with other subroutines and follow an M2, M30 or M99 so it is not reached directly by the flow
of the program.
The L word (or optionally the Q word) gives the number of times that the subroutine is to be
called before continuing with the line following the M98. If the L (Q) word is omitted its value
defaults to 1.
By using parameters values or incremental moves a repeated subroutine can make several
roughing cuts around a complex path or cut several identical objects from one piece of material.
Subroutine calls may be nested. That is to say a subroutine may contain a M98 call to another
subroutine. As no conditional branching is permitted it is not meaningful for subroutines to call
themselves recursively.
7.8.8
Return from Subroutine – M99
To return from a subroutine program: M99. Execution will continue after the M98 which called
the subroutine.
Use M47 to start program execution from the first line again.
Using Tormach PCNC 1100 Series 3
7-34
32397 Rev C1-2
Programming language reference
7.9
Application Defined M-codes
7.9.1
Self-reversing Tapping Cycles
To use the Tormach Auto-reverse tapping heads program M871 P~ (or M872, M873,
M874)
The P word specifies the depth to be threaded relative to the current Z position which will
typically be just clear of the workpiece surface. The P word can be negative or positive with the
same meaning.
Before use of these codes the size of tapping head to be used and the pitch of the thread must be
defined in the appropriated place on the Settings screen. If the part program is running in Inch
(G20) mode then the pitch is taken as a number of threads per inch. If it is metric (G21) then the
pitch will be in millimeters. If the spindle speed is too high for the chosen pitch then an error
message will be displayed and the cycle will not be performed.
The cycle operates as follows:
The currently set spindle speed and thread pitch are used to calculate the feed rate required to
move the tap at the correct speed. The corresponding feedrate for the high speed retraction of
the tap is also calculated. If this exceeds the available rapid rate then an error is displayed.
The tap is then fed downwards for the commanded depth (P word).
At the end of the down-feed the spindle is rapidly retracted by the appropriate distance for the
size of the head in use. This engages the reverse drive.
The spindle is then retracted, at the higher reverse rate previously calculated, for a distance
sufficient to ensure the tap springs clear of the hole.
The Z axis is then positioned at the original height above the work ready to move to another
hole or another tool and operation.
Note:
7.9.2
•
The above explanation is slightly simplified from the actual code used to aid
understanding.
•
For best results, especially for deep holes and blind tapping, the spindle speed chosen
should be checked with a tachometer to ensure it is as near the commanded (S word)
speed as possible.
Goto Toolchange Position – M998
Execution of M998 will send the machine to the tool change position. The tool change position
is defined on the Settings screen. The Z-axis will move first, then X and Y. An entry of 9999
will disable the axis. Execution of this function requires the machine to be referenced (Homed).
7.9.3
User Defined M-codes
If any M-code is used which is not in the above list of built-in codes then the Control Software
will attempt to find a file named “Mxx.m1S” in the Macros folder corresponding to the current
XML profile name. If it finds the file then it will execute the Visual Basic script program it
finds within it.
New macros can be written using an external editor program like Notepad and saved in the
Macros folder.
32397 Rev C1-2
7-35
Using Tormach PCNC 1100 Series 3
Programming language reference
7.10
Other Input Codes
7.10.1 Feed Rate – F
To set the feed rate, program: F~.
Depending on the setting of the Feed Mode toggle the rate may be in units-per-minute or unitsper-rev of the spindle.
The units are those defined by the G20/G21 mode.
Depending on the setting in Configure>Logic a revolution of the spindle may be defined as a
pulse appearing on the Index input or be derived from the speed requested by the S word or Set
Spindle speed DRO.
The feed rate may sometimes be overridden as described in M48 and M49 above.
7.10.2 Spindle Speed – S
To set the speed in revolutions per minute (rpm) of the spindle, program: S~. The spindle will
turn at that speed when it has been programmed to start turning. It is OK to program an S word
whether the spindle is turning or not. If the speed override switch is enabled and not set at
100%, the speed will be different from what is programmed. It is OK to program S0; the
spindle will not turn if that is done.
It is an error if: The S number is negative.
7.10.3 Select Tool – T
To select a tool, program: T~, where the T number is slot number for the tool. The tool is not
changed automatically. It is OK, but not normally useful, if T words appear on two or more
lines with no tool change. It is OK to program T0; no tool will be selected. This is useful if you
want the spindle to be empty after a tool change. It is an error if:
Using Tormach PCNC 1100 Series 3
7-36
32397 Rev C1-2
Programming language reference
•
7.11
A negative T number is used or a T number larger than 255 is used.
Order of Execution
The order of execution of items on a line is critical to safe and effective machine operation.
Items are executed in the order shown in figure 7.5 if they occur on the same line.
If you wish to impose a different order (e.g. to turn coolant off before the spindle is stopped)
just code the commands on separate blocks.
7.12
Error Handling
This section describes error handling in the Control Software.
The Control Software sometimes ignores things that it does not understand. If a command does
not work as expected or does not do anything, check that you have typed it correctly. The
Control Software does not check for axis over travel or excessively high feeds or speeds. Nor
does it does not detect situations where a legal command does something unfortunate, such as
machining a fixture.
Order
1
2
3
4
5
6
7
8
9
10
11
12
13
14
15
16
17
18
19
20
21
Item
Comment (including message)
Set feed rate mode (G93, G94, G95)
Set feed rate (F)
Set spindle speed (S)
Select tool
Tool change (M6) and Execute M-code macros
Spindle On/Off (M3, M4, M5)
Coolant On/Off (M7, M8, M9)
Enable/disable overrides (M48, M49)
Dwell (G4)
Set active plane (G17, G18, G18)
Set length units (G20, G21)
Cutter radius compensation On/Off (G40, G41, G42)
Tool table offset On/Off (G43, G49)
Fixture table select (G54 – G58 & G59 P~)
Set path control mode (G61, G61.1, G64)
Set distance mode (G90, G91)
Set canned cycle return level mode (G98, G99)
Home, change coordinate system data (G10) or set offsets (G92, G94)
Perform motion (G0 to G3, G12, G13, G80 to G89 as modified by G53
Stop or repeat (M0, M1, M2, M30, M47, M99)
Table 7.5 – Order of execution of commands on a line
32397 Rev C1-2
7-37
Using Tormach PCNC 1100 Series 3
Machine upgrades and configuration
8.
Machine Upgrades and Configuration
8.1
Fourth Axis – Rotary Table
The fourth axis can be used as a rotary table (i.e., with its axis of rotation parallel to the Z-axis)
or more commonly as a dividing/indexing head with its axis of rotation parallel to the X-axis.
8.1.1
Installing the Electronics
Full details for installing the electronics and setting up the rotary table can be found in the
Tormach 4th Axis and Rotary Products Manual (RotaryProducts_UM.pdf). This comes with
every Tormach 4th axis Kit and is also available to download from our website,
www.tormach.com.
8.1.2
Utilizing the Fourth Axis
8.1.2.1
Referencing and Zeroing the Fourth Axis
The Tormach rotary table does not have a built-in home switch. When you are setting it up, if
the initial position is important, then you should use the + and - keys on the numeric keypad to
jog it into position. When in a suitable position click Zero A. This will set the A DRO to zero in
the current work offset system. If you use multiple work offsets then you should Zero A in all of
them.
It is possible to provide a home switch in conjunction with a fixture on the fourth axis and
interface it to the PCNC using the Accessory socket on the control panel. In this case the Ref A
button can be used to move to this switch in the same way as the linear axes. If you do this
accidentally, with no switch connected, then the movement can be cancelled with the Esc key.
8.1.2.2
Diameter Compensation Feature
To understand this it is useful to recall what happens on a G01 (line) move where two axes like
X and Y are coordinated. The control software will attempt to move along the line at the feed
rate requested by the F-word (or DRO). For example a move at a feed rate of 10 inches per
minute from X = 0, Y = 0 to X = 1.0, Y =
1.0 will move both the X- and Y-axes at
about 7 inches per minute. By Pythagoras’
Theorem the diagonal speed is √(72 + 72) =
9.9.
Now if a move of X needs to be coordinated
with one of A there is a problem because A
moves in degrees. We only know how fast
the tool is moving through the material if we
also know the diameter of the part in the
rotary axis. The Control Software will take
this value from the Rotational Diameter
DRO on the settings page.
Note: This feature only applies to
coordinated moves. A single G01 move of
the A-axis will use the feed rate defined by
the F word as a number of degrees per
minute.
Figure 8.1 – Engraving on a cylinder
32397 Rev C1-2
8-1
Using Tormach PCNC 1100 Series 3
Machine upgrades and configuration
8.1.3
Fourth Axis Applications
General use of a fourth axis requires CAD/CAM software that will create a part-program using
the A-axis but useful work can be done with three axis software.
8.1.3.1
Engraving on a Periphery of a Cylinder
If you can engrave in X-Y with a Wizard or CAD/CAM software then it is easy to adapt an XY part-program to use the fourth axis (figure 8.1).
The rotary table is mounted with its axis parallel to the X-axis. The work to be engraved is
mounted on a mandrel supported by the tailstock. It is of course important that it runs true or
the depth of the engraving will be uneven.
The engraving is prepared as if it to be engraved in the X++ direction (i.e., the height of the
letters is movement of Y). The code may not use G02 or G03 (arc) commands.
There are then three stages in engraving on the cylinder: (a) the part program is converted to be
motion in A and X instead of X and Y; (b) the A motion is scaled to convert it to degrees; and
(c) the radius of the cylinder is defined to ensure the correct feed rate on the surface being
engraved.
Editing the Part-program
Load the X-Y engraving part-program for
your text. Click the Edit button in the file
control family. Use the Replace function of
the edit to change all instances of “X” to “A”
and then all instances of “Y” to “X.” This
orients the engraving (figure 8.1).
Scaling the “Width” of the Text
The original part-program will move along
Figure 8.2 – Scale and Radius Correction
the engraving in linear units (e.g., inches) but
now it is edited to use degrees, the A-axis needs scaling. If the radius of the cylinder is R (mm
or inches depending on what the control program is set in) then the A-axis scale should be set to
57.3 ÷ R (i.e., 360 / (2 π x R)). For example, the radius of the disk in figure 8.1 is 1.21" so the
scale for A was set to 47.36 by typing this value into the A Scale DRO on the MDI screen
(figure 8.2).
Figure 8.3 – Gear cutting
Figure 8.4 – Gear cutting (tailstock removed for
clarity)
Using Tormach PCNC 1100 Series 3
8-2
32397 Rev C1-2
Machine upgrades and configuration
Setting the Radius Correction
If you are using this improvised sort of code for a fourth axis then you must set the Radius
correction DRO which is on Settings and also the MDI screen to an estimate of the radius of the
part mounted in the axis (figure 8.2). This ensures that the feed rate will be correct.
8.1.3.2
Gear Cutting
Figures 8.3 and 8.4 show the fourth axis set-up for cutting a spur gear.
The G-code for this is easily produced by hand or by a Wizard as it consists of a series of
passes cutting a tooth followed by indexing by an angle (say A) corresponding to the number of
teeth (N). A = 360 ÷ N .
It is important that the gear cutter is exactly on the centerline of the gear and its mandrel. A
Figure 8.4 – Gear cutting (tailstock removed for
clarity)
Figure 8.5– Ruler vertical so on center
Figure 8.6 – Ruler tilted to left at
top so cutter is too high
steel rule can be used to set this quite accurately (figures 8.5 & 8.6).
The rule can be seen against the body of the chuck above the mandrel.
Notice that the test is more sensitive the smaller the diameter of the object onto which the rule
is placed, so the setup is done on the mandrel not on the gear blank itself.
If the gear cutter is mounted so that it can be inserted at the same height each time (e.g., on an
R8 holder), then it may be worthwhile to set-up and save a work offset giving the centerline as
32397 Rev C1-2
8-3
Using Tormach PCNC 1100 Series 3
Machine upgrades and configuration
Y=0.0 and Z=0.0 so that the setup does not need to be
repeated each time the machine is switched on.
8.2
Probes (Active and Passive) and Tool
Setters
8.2.1
Introduction to Uses of Probes and Tool
Setters
If you mount a switch in the spindle instead of a cutting
tool and connect the switch to the control computer so that
the software can "read" it, then you can use the machine
for measuring instead of cutting. The switch is usually
arranged so it operates when a probe tip is moved
horizontally in any direction or pushed up. Figure 8.7a
shows a probe from the Tormach range of accessories (p/n
30668) probing the top of a partially machined part.
Figure 8.7a – Tormach probe
The Tormach probe has a standard TTS (¾") shank and is
best used in the ¾" R8 collet (p/n
30146).
Note: We advise you to mark the
spindle pulley with a dot of paint
and always to insert the probe with
the spindle in the same position.
This eliminates any errors caused by
random positioning. Keep the
spindle lock ON when the probe is
in. This will prevent any accidental
startup of the spindle motor which
would rip the cable out of the probe
body.
Figure 8.7b Some probe packaging options
A Renishaw or other standard probe can be
interfaced using an appropriate cable. Interface
details are given below.
The other possibility is to have a tool in the spindle
and "replace" the work with the switch. This allows
measurement of the length of the tool and setting the
coordinates of the plane on which the switch is
standing. Figure 8.8 shows the Tormach Tool Setter
(p/n 30669) in use on a tooling plate.
There are two main uses for the measurements
taken:
(a) They can be used to set up the offsets in the
Control Software so that the cutting defined by the
part program is in the correct place relative to the
stock material or part machined component
(b) They can be recorded to allow the shape of an
existing model object to be input to a computer
aided design (CAD) program.
Figure 8.8 – Tormach toolsetter
We refer to the first application as probing and the second as digitizing.
Using Tormach PCNC 1100 Series 3
8-4
32397 Rev C1-2
Machine upgrades and configuration
Note: Our Probes and Tool setters have changed in
appearance a bit from the ones pictured in the following
sections. All instructions and descriptions still apply.
8.2.2
Probing for Work/Tool Setting
The basic operation of the probe is controlled by the G31
code (q.v.). In practice you will not want to write
programs to set up a job so a series of interactive screens
is provided to perform probing operations. These are
divided into measuring (probing) X and/or Y positions
and probing Z positions. To make effective use of these
screens you need a basic understandings of the concepts
of Work Offsets and the Tool Length offset. You will
have used Work Offsets already in setting up any work
on the table even if only unconsciously by using the axis
Zero buttons.
Figure 8.9 – Data for Probe (T#99)
The screen buttons all use the current feedrate (F DRO). We recommend using 20 IPM.
As they do not involve Tool length offsets we will describe the X/Y Probing screen first.
Before this there is one bit of configuration to do.
•
Locate the effective diameter of your probe tip (usually made of ruby to avoid wear) in
the inspection certificate supplied with the probe. The standard tip diameter is around 4
millimeter (0.1575")
•
Enter this diameter for Tool #99 on the Offsets screen (figure 8.9). Ignore the Length for
now and if it is zero then the Offset On/Off LED will not be lit. This is unimportant.
Note: The geometry of probing is complex and the certified effective diameter will be different
from the actual diameter that you can measure.
8.2.2.1
Simple X/Y Probing
This screen (figure 8.10) allows you to set the origin (X = 0.0, Y = 0.0 point) to some feature of
the stock material or a partly finished component.
The three pictures represent the three operations on this screen. (a) Finding center of a bore, (b)
Finding a plane surface and (c) Finding the corner of the fixed jaw of a vise. The convention is
on all screens is that a
yellow screen button
will make the PCNC
move the probe
looking for the part.
Obviously two things
are necessary. The
probe must be plugged
in to the socket on the
PCNC control panel
(and hence be
connected to the
computer) and the Z
height must be low
enough so the probe
tip will actually touch
the work.
Important: If the
probe is not properly
32397 Rev C1-2
Figure 8.10 – Simple XY Probing
8-5
Using Tormach PCNC 1100 Series 3
Machine upgrades and configuration
connected then the Control Software will keep moving even when the probe touches the work.
This can cause it to be bent. Each time that you connect up the probe you should check that the
screen LED marked Test probe before use lights when you gently displace the tip. The red
lights in the probe will illuminate too but the screen LED is a more complete test.
We strongly recommend use of the Jog/Shuttle controller for jogging the probe position.
because it combines precision with speed. If you hit anything while jogging the machine does
not stop and, although the probe tip has a lot of over-travel, there is a risk of bending it or
breaking the ruby tip.
You are also advised to set the current tool number to 99 when you insert the probe into the
spindle. This ensures that the correct offsets are used by the Control Software whatever
sequences of moves you perform.
Bore Center
Jog to position the probe tip so it is just below the top surface of the bore to be probed and
anywhere roughly near the center. No precision is needed in this position. Click the Find Center
and Set work origin button.
The probe will make three pairs of exploratory moves. First it goes left and right (X – then
X++) and so estimates the X coordinate of the center. Then it goes to the estimated X-center
and probes back and forward (Y—and Y++). This gives the exact Y center. Finally, using this,
it refines the X center by the final pair of moves (The initial X moves off the Y center could
have been slightly inaccurate because of the oblique contact of probe tip with the bore).
Then the current work offsets (typically by default the G54
system) are set so the bore center is 0,0 (the X/Y origin). As the
probe tip is in the center the X and Y axis DROs will read 0.0.
Position of a Face
You can set the X origin of a plane face perpendicular to X or the
Y origin of a plane face perpendicular to Y. The Yellow buttons
X+, X-, Y+ and Y- determine which direction the probe will move.
You should start within ½" or so of the face and with Z low
enough so the tip hits the face.
Figure 8.11
After the probe trips it moves slightly away from the face that it has found and the control
software sets the corresponding current work offset so that the face is coordinate 0.0. This is
typically useful to set the two edges of a piece of material to be the origin of their axes (i.e. the
corner will be 0.0, 0.0)
There are occasions when you actually want to set both X and Y offset values to the location of
the point probed. To do this toggle the green button Set X AND Y before making the probe
move (figure 8.11). Two different moves will not, of course, be meaningful if they use "Set X
and Y" as the second overrides the first.
The probed face should not be
significantly angled to the X or Y axes
and should be flat. Any errors here will
be reflected in the accuracy of the
probed position. If you need to probe
inclined and/or radiused faces then you
need to look at the Comprehensive X/Y
Probing screen.
Corner of Vise
It is very quick, for machining a small
batch of parts that can be held in a vise,
to align the stock by feel to the corner of
the fixed jaw. This function allows you
Using Tormach PCNC 1100 Series 3
Figure 8.12 – Vise jaw corner
8-6
32397 Rev C1-2
Machine upgrades and configuration
to find the back left corner which is a typical choice for X = 0.0 Y = 0.0.
Jog the probe to ¼" to ½" down and to the left (South-West) of the corner of the fixed jaw. The
Z height make the probe tip be below the top of the jaws. Set the Jaw width DRO to the size of
your vise (this will be remembered for subsequent uses of the screen)
The probe explores using the three moves shown on the screen panel (figure 8.12)
Move 1 establishes the rough position of the jaw. Move 2, near the far end establishes the angle
the vise is mounted at (and displays it in the DRO). Move 3 approaches the end of the jaw
(along a perpendicular). The X/Y origin of the current work offsets is then set to the calculated
position of the corner and the probe moves to its starting point.
The angle DRO
gives you a
confidence check the
setup accuracy of
your vise. If it is a
long way from 0.0
degrees then Move 2
might not find the
jaw (or might even
hit the moving jaw).
If you need to work
with a significantly
skewed vise or to
very close tolerances
then the
Comprehensive X/Y
probing screen has
features that will
help.
Figure 8.13 – Z Probing screen
Notes for all
operations: You can use these operations with a part program loaded or indeed with one partly
run (say to an optional stop). The probing will
however set the Control Software to Absolute
Coordinates (G90), No rotation (G69), No axis
scaling (G50) and cancel canned cycles (G80)
8.2.2.2
Z Probing
Figure 8.13 shows the Z probing screen. It has two
distinct functions depending on whether the probe is
in the spindle or a normal tool is in the spindle and
the tool setter is connected to the probe input.
The yellow buttons perform machine moves and set
offsets. Depending on the button, these will be the Z
offset in the current work offsets or the length of a
tool.
Important: If the probe or tool setter is not properly
connected then the Control Software will keep
moving even when the probe touches or the setter is
touched. This can cause the probe tip to be crushed
or the cutting edges of the probing tool to be
chipped on the carbide top of the setter - the PCNC
is very powerful! Each time that you connect up the
probe or tool setter you should check that the screen
32397 Rev C1-2
8-7
Figure 8.14 – Probing Z
Using Tormach PCNC 1100 Series 3
Machine upgrades and configuration
LED marked Test probe before use lights when you gently displace the tip or cap. The red
lights in the device will illuminate too but the screen LED is a more complete test.
We strongly recommend use of the Jog/Shuttle controller for jogging the probe position.
because it combines precision with speed. If you hit anything while jogging, the machine does
not stop and, although the devices have some over-travel, there is a risk of damage.
Probing a Z Surface
If the Control Software knows the length of the probe relative to the master tool then you can
set the current work offset so any surface you probe is Z = 0.0; conversely if you have a Z = 0.0
surface then you can set the length of the probe in the tool table. The pane that does this is
shown in figure 8.14.
We describe setting the tool length first although it needs to be done very infrequently (e.g. if
the probe tip is changed or the master tool length has to be altered). The yellow button is semitransparent to reflect the infrequent use and visually draw you to the Set Work Offset button.
•
Put the master tool in the spindle and type its number (traditionally tool #0 or #1) into
the T DRO. Jog Z so it just touches the table or any flat Z surface. Zero the Z axis DRO.
You can use this or any of the standard setup processes for the Z work offset (for details,
revise offsets and in particular sections 6.1 and 6.3)
•
Load the probe into the spindle
•
Click the button Move and Set Tool length so the probe trips on the same surface you
used to touch the master tool. This will set the length of Tool #99 (the probe) relative to
the master tool.
In everyday running you can now set any surface to be Z = 0.0. Just put the probe tip above the
surface that is to be Z = 0.0 and click Move and Set Work Offset. This is the best way to set the
Z work offset if the probe is in the spindle for setting X and Y too.
Setting a Tool or Z Surface
The other pane on the Z probing screen is used with the tool setter. It is shown in figure 8.15.
Here there are three quantities and provided two are know the third can be quickly set. The
height of the tool setter sensor is essentially a constant so needs to be put into the DRO once
after each installation or upgrade of the Control Software.
We first describe setting the sensor
height.
•
Put the master tool in the spindle
and put its number in the Tool #
DRO
•
Touch it on a flat Z surface like
the table of tooling plate and set
the current work offset so Z = 0.0
( sections 6.2 and 6.3 give a range
of methods).
•
Jog the master tool so it is above
the sensor. Tests its wiring by
depressing the top and checking
that the Test Probe before move
LED lights and click the Setup
Sensor Height button. This will
set the persistent DRO recording
the sensor height.
To set tool lengths in the tool table you
work as follows:
Using Tormach PCNC 1100 Series 3
Figure 8.15 – Tool setter
8-8
32397 Rev C1-2
Machine upgrades and configuration
•
Select the master tool. Touch a Z surface with the master tool and set work offset so Z =
0.0 as above.
•
Put the number of the tool you are measuring into the Tool# DRO and put the tool in the
spindle.
•
Click the Setup Tool Length button. The tool will move and be sensed by the setter and
its length relative to the master tool be entered in the tool table.
To set a plane as Z= 0.0 with a given tool
•
Load the tool in the spindle and put its number in the Tool# DRO
•
Place the Tool Setter under the tool on the surface to be made Z = 0.0
•
Click the Setup Work Offset button. The tool will move down onto the setter and the
work offset will be reset.
Notes:
(a) If the setter is not directly under the tool then the probing move will miss the setter and so
continue until the tool hits the table or fixture. If you see this happening trip the sensor by hand
or use EStop to abort the move.
(b) You can use the Setup Work Offset button, and the
setter, for tools held by a system like ER collets where
you do not know the tool length. You must set up the
setter height correctly but then click Setup Work Offset
whenever you change a tool. In this case the tool length
does not matter – everything is done by the Z work offset.
You must not mix this method of working for some tools
with using the tool table for others because of the
differing use of the work offsets in the two methods.
8.2.2.3
Figure 8.16 – Accessing the Comp
Probing screen
Comprehensive X/Y Probing
The simple X/Y probing screen is designed so that the one click does everything needed to set
the required offsets. This imposes the limitation that the moves are performed by the software
rather than by the operator. For example while you can find the center of a circular bore you
cannot find the center of a circular protruding boss even though the basic geometry is identical.
A Comprehensive Probing screen is provided to overcome this limitation. The screen is
accessed by a button on the simple X/Y probing screen (figure 8.16).
Figure 8.17 shows the Comp X/Y Probing screen.
It gives the operator the required flexibility by separating the actions of probing for feature on
the work and setting work offsets from the features. The interface between the operations is the
X/Y coordinates of three points which are stored and displayed in a bank of DROs.
32397 Rev C1-2
8-9
Using Tormach PCNC 1100 Series 3
Machine upgrades and configuration
Figure 8.17 – The two areas of Comp X/Y Probe screen
The probing and recording function is done using the yellow buttons and the DROs enclosed in
the red box of the figure. The offset setting is done with the DROs and green buttons enclosed
in the blue box.
Probing to Set Point DROs
Before probing you should set which Point will be used to record the probed coordinates by
clicking Select 1, Select 2 or Select 3. The adjacent LED will indicate the currently selected
point.
The circular central yellow button will set the Point to the centre of the circular hole in which
the probe tip is placed. Ensure that the Z axis is lowered sufficiently so contact is made on the
"equator" of the tip.
The cross-pattern of square buttons probes in the two X directions and the two Y directions.
Unlike on the simple X/Y Probing screen, the face being probed does not need to be square-on
to an axis and can be a circular arc segment. This is indicated by the graphic on the buttons.
The angle and possibility of an arc are detected by making a main probe move followed by two
side-steps 0.2" either side of the main move. The coordinate recorded in the selected Point
DROs is the point where the main move contacts the work. The diameter of the probe tip is
allowed for so, as for simple probing, it must be correctly entered for tool #99 in the tool table.
The probe is returned to its initial point.
Progress of the operation is noted on screen in the message line. If Verbose Messages are
selected (indicated by the LED next to the toggle button) then details of what the probe found
will be given. If the face has a radius of curvature of greater than or equal to 20" the angle of
the face (or tangent to the large circle it is part of) will be given. If the radius of curvature is
less than 20" then an estimate of the radius and the center point will be displayed. Clearly these
will not be particularly accurate as they are derived from three points that are very close
together but this information can be a useful check on the setting of the work.
Using Tormach PCNC 1100 Series 3
8-10
32397 Rev C1-2
Machine upgrades and configuration
When one point has been probed then another can be selected and the DROs set by probing
another feature.
In some situations you may not need to probe to
set the Point DROs. You can just type values into
then (followed of course by Enter). Point 1 can
also be zeroed by a button.
Figure 8.18 shows probing for three points to find
the center of a feature that could not be located by
the simple X/Y Probing screen.
Setting Offsets from Points
Once you have a point or some points you can use
them to set work offsets by using the green
buttons.
Figure 8.18 – Finding a tricky center
Origin X, Y, or X and Y from a point: The buttons outside the circle use just one point. If you
only want to set the X offset use Point 1. If you want to set just the Y offset use Point 2. To set
both X and Y use Point 3.
Origin X and Y are center of an arc: Set all three Points to lie on the circle or arc. Click the
Origin is Center button. Although the picture on the screen implies the points are roughly
equally spaced around the circle, and this will give the greatest accuracy, you can work with a
small segment of arc drawn from a large circle whose center is outside the machining envelope
by many feet. As the points can be centers of holes it can find the center of a set of holes on a
pitch circle like a pipe flange.
Origin X and Y are at intersection of line and
perpendicular from a point: Again you set all
three Points. Points 2 and 3 define the line and
Point 1 from where the perpendicular is to be
dropped. Click the Origin is "corner" button.
The picture implies that the perpendicular should
intersect the line between the probed points but
this is not necessary. The "corner" can be on any
projection of the line. This function is a
generalization of the vise jaw locator on the simple
screen. It can set the origin to any corner of an
object in any orientation.
Setting Rotation from Points
This function is used to set up the machine to mill
components where the X/Y axis of the part is not
Figure 8.19 Probing Point 2 – Cable right
square to the X/Y axis of the machine. This might
be because the part does not have any square faces accessible when it is mounted for a second
operation. The function uses the G68 code to rotate the working coordinate system relative to
the machine coordinate system. You should be sure you understand the working of G68 by
running test pieces before you use it on a job.
Point 1 defines the center of rotation in the existing work coordinates. It is often convenient to
keep this as 0,0 or for it to be the same as one of the other points. Points 2 and 3 define a line
whose angle is the direction of the new coordinate system.
If no flat face is accessible it will often be useful to have Points 2 and 3 as the centers of holes
already drilled or bored in the part.
32397 Rev C1-2
8-11
Using Tormach PCNC 1100 Series 3
Machine upgrades and configuration
Click the button Axes to set the G68 command. The angle of rotation used is displayed in the
DRO and if it is non-zero the LED on this screen and next to all axis DROs will indicate that
G68 is active. The X and Y DROs will be red to
remind you the rotation is active.
Rotation is removed by clicking the Clear Rot
button, by typing 0 into the angle DRO or by using
a G69 command.
8.2.2.4
Probe Calibration
For the probe readings to be meaningful the center
of the probing tip ball needs to lie on the centerline
of the spindle. The Tormach probe has three set
screws which are used to adjust this alignment.
Most other probes will have similar features
although the pitch of the threads and the orientation
of the screws may differ and so require alteration to
the details of this procedure.
To align the probe tip you need a hole about ½"
diameter and ¾" or so deep machined in a block of
material so that it is perpendicular to the bottom
face of the block.
Figure 8.20 – Point 3 – Cable left
The hole should be as circular as possible so ideally be reamed or bored on a lathe. If it is
produced on a lathe then having a through hole and facing the end provides the accurate bottom
face. A rough setting can be made using the TTS Measurement Fixture (p/n 30140) although its
bore is not finish machined.
•
•
Insert the probe in the machine spindle (in the collet with which it will be used) so that
the connector and cable are on the
right (X ++) direction. Leave the
spindle lock on.
•
Work using the Comp X/Y
Probing screen. Zero the Point 1
DROs as it is not used. Select
Point 2 and use the round yellow
centre finding button to record the
center of the alignment bore. This
is illustrated in figure 8.19.
•
Rotate the spindle by half a turn
and re-lock it. The cable will now
be to the left (figure 8.20)
•
Select Point 3. Again use the
round yellow button to find the
Figure 8.21 – Controls for probe alignment
center of the alignment bore. If the
probe was perfectly set points 2 and 3 would be coincident. They probably will not be so
you need to know how to adjust the screws.
•
Rotate the probe back to the Cable Right position.
Click the Adjust Probe from 2 and 3 button. The message line will display the movement
required on the three screws to centralize the probe tip.
o
On the active probe, the screw opposite the connector and cable is Screw
1 and the others number clockwise looking from the top. So Screw 2 is
facing the control cabinet and Screw 3 is visible on the "southeast" side
of the probe. The numbers are included on the probing photographs
Using Tormach PCNC 1100 Series 3
8-12
32397 Rev C1-2
Machine upgrades and configuration
above for additional clarity. A positive number is tightening the screw
and a negative number loosening it. The value is millimeters which
equates to turns on the Tormach probe. You must loosen the screw(s)
first then tighten the other(s).
On the passive probe, the adjustment screws are the small Allen set
screws. The larger socket head cap screws are retaining screws, which
need to be loosened at least 1‐2 turns before adjusting the set screws. The
set screw under the connector is Screw 1, and the others number
clockwise when looking from the top. Screw 2 faces the operator’s left,
Screw 3 faces the mill column. Like the active probe, a positive number
is tightening the screw and a negative number loosening it. You must
loosen the screw(s) first then tighten the other(s).
You will not be able to estimate, say, 0.11 turns so get as near as you can and repeat the
procedure getting nearer and nearer to the ideal point where all screw movements are
zero. For most purposes 0.03 of a turn which is about 0.001" will be good enough.
o
•
•
8.2.3
Make sure all the screws are tight and re-check the calibration.
Digitizing parts from a model or for reverse engineering
Details of the software for this will be published in a later revision on this document.
8.2.4
The Probe Electrical Interface
Figure 8.22 – PCNC1100 Interface to probe
Probes are connected to the auxiliary socket is provided on the operators control panel. This can
be used for interfacing any device that needs an input that can be read by the Control Software.
It can be used for user supplied devices. The exact interfacing will depend on the device to be
used but the following description of the available signals will allow liaison with the device
supplier/designer.
The interface is presented as a 5 pin DIN socket. The pin assignment is:
Pin number 1 is +5 Vdc, useful if you have to bring power to active electronics on a probe.
Pin number 3 is +12 Vdc, useful if you need to supply power to active electronics on a probe.
Pin number 4 is logic ground. Do not attach to the machine ground (i.e., your probe casing
should be isolated from this ground).
32397 Rev C1-2
8-13
Using Tormach PCNC 1100 Series 3
Machine upgrades and configuration
Pin number 5 is the signal. It is internally pulled up to 5 volts in the PCNC. The input is active
(“on”) when this is pulled to ground. Thus by jumpering 4 to 5 and you will see the probe LED
change on the Diagnostics screen.
8.2.5
Other
There are a number of other tools available that are less integrated than those described in this
chapter, but are designed to accomplish similar tasks, such as our Haimer® edge finders,
rotating lighted edge finders, tool length
touch off tools and off line tool length
measurement devices . Please review our
full Tormach Tool System (TTS) catalog,
DS_TTScatalog-2.pdf, for more
information.
8.3
Auto-reverse tapping
The control software supports auto-reverse
tapping heads supplied as accessories to the
PCNC. PN 30612 ranges from #0 to ¼"
threads and PN 30613 covers #8 to ½". The
DROs on the Settings screen are used to
define the head in use and thread pitch. The
actual threading commands M871, M872,
M873 and M874 are described in chapter 7.
This section gives brief instructions of
fitting the heads to the machine and
Figure 8.23 – Large tapping head ready for use
installing a tap.
Both tapping heads are supplied with the
Tormach Tooling System geometry
whose ¾" shank can be mounted like
any other tool.
Figure 8.23 shows the large head fitted
in the spindle. The torque arm can be
seen engaged in the recess in the head
casting to prevent rotation on the fixed
part of the mechanism. Tapping will
generally be performed between 500 and
900 RPM so the drive should be set to the
low speed pulleys.
The tap is held by a rubberflex collet locked
by the nut on the nose of the head spindle
and prevented from rotating in the head by
using its squared end. The small head
accepts a fixed square but the larger head,
which covers a bigger range of sizes, has a
set of alternative blocks which fit into a
square hole above the collet nut. The tap
holding arrangement, without the spindle is
shown in figure 8.24 and the accessories for
the large head are shown in figure 8.25.
This picture also shows the square hole in
the tapping spindle which houses the antirotation block.
Using Tormach PCNC 1100 Series 3
8-14
Figure 8.24 – Tap collet and anti-rotation block
Figure 8.25 – Accessories for large
tapping head
32397 Rev C1-2
Machine upgrades and configuration
The top ring on the tapping head should be screwed down to give the highest tapping torque. As
the machine is applying the feed any rotational slippage will cause problems.
(1) Tapping can be done using the M871 (M872 etc.) cycles, tapping code generated by CAM
systems such as SheetCAM and, of course, hand written G-code. The recommended sequence
is the same in each case (figure 8.26):
•
Feed the Z axis down at a rate corresponding to the pitch of the thread and the spindle
speed. The distance of this move will be the depth to be tapped plus the initial Z
clearance.
•
Rapidly retract the tapping head. As the tap is held in the thread this will pull the spindle
out of the head and engage reverse gear.
•
Feed the Z axis up at a rate corresponding to the pitch of the thread and the (geared up)
speed of the reverse running tap. The distance of this move should be sufficient to
ensure the tap completely leaves the thread.
•
Optionally position the Z axis at the initial Z clearance height.
Figure 8.26 – Moves in tapping a hole
(2) The M871 (M872 etc.) cycles also offer an alternative algorithm which is slower, may cause
more wear on the tapping head, but allows more accurate control of depth and so is suitable for
tapping blind holes.
•
Feed the Z axis down at a rate corresponding to the pitch of the thread and the spindle
speed. The distance of this move will be the depth to be tapped minus the distance that
the head needs to be extended for the clutch to disengage plus the initial Z clearance.
•
Pause for 2 seconds. The rotating tap will be pulled into the work by the existing thread
until the clutch disengages. This depth in independent of speeds or feeds. The tap stops
rotating and stays at the de-clutch depth.
•
Feed the Z axis up at a rate corresponding to the pitch of the thread and the, geared up,
speed of the reverse running tap. The distance of this move should be sufficient to
ensure the tap completely leaves the thread.
•
Optionally position the Z axis at the initial Z clearance height.
Notes:
32397 Rev C1-2
8-15
Using Tormach PCNC 1100 Series 3
Machine upgrades and configuration
It is usual to underfeed slightly in both directions (2% to 5%). This might result in the clutch
disengaging but it is better than hitting the stops on the retractable spindle.
The choice of a suitable tap designed for machine tapping is important. Conventional taps for
manual use are unlikely to give satisfactory results except on shallow depths with easy to
machine materials.
The exact depth fed in method (1) depends on the accuracy and stability of the spindle speed.
This makes tapping blind holes where the thread depth is nearly as deep as the drilled hole, a
process which requires experiment to get the optimum depth. (2) is an alternative feed strategy
which can increase the accuracy of tapping depth with the trade-off of greater wear on the
tapping head clutch.
In tapping blind holes, it is common practice
to rough tap by machine and then clean the
hole and the bottom the thread with a handheld tap or pneumatic power head.
If you are writing your own G-code, the rapid
retraction is best done by a G01 move with a
large feedrate (say F99999) as this ensures
that the control software Constant Velocity is
used to make the fastest and smoothest
reversal. CV would not be used if G00 is
employed.
In method (1), during the start of the rapid
retraction the tap is still actually moving into
the hole and not stationary. This should be
allowed for when calculating distances.
Figure 8.27 – Measuring spindle speed
For best results, especially with long threads, you should check that the actual spindle speed
corresponds to that commanded by the S word by using a tachometer (e.g. Tormach p/n 30527)
(figure 8.27).
It is not advised to use the "Pause" feature in Mach3 during a tapping routine.
For more information on tapping, please review our tapping guide called
"TD_tapping_Guidelines-4.pdf" available on our website, www.tormach.com.
In addition to the Auto Reversing Tapping head, Tormach also offers a fully featured
Tension/Compression (or "Floating") tapping head. . Please review our full Tormach Tool
System (TTS) catalog, DS_TTScatalog-2.pdf, for more information.
Figure 8.28 – Compression tapping head
Using Tormach PCNC 1100 Series 3
8-16
32397 Rev C1-2
Warranty, Specifications, Customization and Troubleshooting
9.
Warranty, Specifications, Customization and
Troubleshooting
9.1
Intended Use Statement
The PCNC is intended for use as a general purpose CNC milling machine. The intended use
includes cutting conventional (non-abrasive) materials such as unhardened mild or alloy steels,
aluminum, plastics, wood and similar materials – in fact any material that can be cut with a
rotating cutter. The PCNC is intended to be used with the software configuration files provided
by Tormach.
9.2
Support
Tormach provides free technical support through multiple channels. The methods are listed
below, in order of preference. The quickest way to get the answers you need is normally
checking in order of preference:
9.3
•
This manual – ALWAYS the first place to check!!
•
Related documents found at: http://www.tormach.com/documents.html
•
Our website at: www.tormach.com
•
Email to: [email protected]
•
Telephone Tormach at: 608-849-8381
•
Fax Tormach at: 209-885-4534
Outside of the Scope of Intended Use
Applications for the equipment or modifications of the equipment outside of the Intended Use
Statement are supported through consulting engineering, not through our free support policy.
There are no limits to the applications that Tormach products can be used for or to the
modifications that can be applied to the Tormach machinery. Tormach designs use standard
industrial components and incorporate the principles of Open Architecture specifically to allow
and promote these variations. With Open Architecture controls, industrial engineers will find
Tormach products cost effective to incorporate into larger manufacturing systems, or with
easily separable base, column and head sections manufacturing engineers looking to design
specialized in-house equipment will find they can use the base as a low cost motorized XY
table. Some machinists may want to convert a stepper mill to servos or some software engineers
may want to replace the Tormach approved software with something of their own creation.
All of the technical information and insight required to support these variations from the
intended use cannot possibly be foreseen. If the extensive documentation provided does not
supply all the information you need, we can provide additional information and engineering
support required for your project on a consulting engineering basis. We are actually very good
at this. If you have your questions well organized we can normally provide all the information
you need in short order. Consulting engineering is done by electrical and mechanical engineers
and billed at current hourly rates.
As you might expect, all warranties for Tormach equipment are voided through modification to
the equipment or use outside of the Intended Use. Individuals or companies involved with
modifying the equipment or applying the products assume all consequent liability.
32397 Rev C1-2
9-1
Using Tormach PCNC 1100 Series 3
Warranty, Specifications, Customization and Troubleshooting
9.4
Specifications
9.4.1
Mechanical
9.4.2
•
Table Size – 34" x 9.5"
•
Table Slots – 2 drainage/alignment slots, 3 T-Slots 0.625" (5/8") – center slot -0.00 +
0.004" – outer slots – 0.000 + 0.008"
•
Travel (X-, Y-, Z-axis) – 18" x 9.5" x 16.5"
•
Spindle Nose Diameter – 3 3/8"
•
Spindle Taper – R8 with spindle lock for easy single hand drawbar operation.
•
Spindle Speed Range RPM – 100 to 5140. Computer controlled spindle speed and direction
with regenerative braking from a 1.5 hp induction motor (2 hp peak).
•
Cartridge style spindle with V-belt transmission. There are two overlapping speed ranges.
Low belt speed is 100 – 2000 RPM, high belt is 250 – 5140 RPM
•
Spindle Center to Column Face – 11"
•
Maximum Weight of Workpiece – 500 lbs.
•
Max spindle nose to table – 17"
•
Forward opening electrical cabinet. This unique design allows service even when the
machine is placed near to a wall.
•
Weight net / shipping. – 1130 / 1325 lbs
•
Operating temperature range 45 to 100 oF (7 to 38 oC)
•
Rapid traverse X, Y = 110 IPM, Z = 90 IPM
•
NEMA 34 stepper motors on X, Y and Z
•
Single Shot Lube Pump
•
15 point lubrication. Each axis has an oil distribution channel milled full length on left and
right vertical and horizontal surfaces (all 4 sliding surfaces) plus an oil line plumbed
directly to the ball nut assembly.
•
Precision ground ball screws in the X, Y and Z motion. ISO/DIN P4 grade.
•
Complete way covers.
•
Slide ways are a bonded low friction surface (PTFE filled acetyl), hand scraped slide ways
with milled oil distribution slots.
•
1 Year warranty. There are no on-site factory service personnel. Warranty service will
involve replacement of components with direction from Tormach support staff.
Electrical
•
Spindle safety is enhanced with a tool change safety interlock and key switch lockout. Main
spindle contactor (VFD power) is automatically disengaged when operator is changing a
tool. Spindle M-codes or manual spindle start will reengage VFD power automatically after
tool change is completed.
•
Operator console has manual override for all spindle controls.
•
PC Windows Control with integrated safety & manual overrides (PC not included,
Windows XP or Windows Vista is required). Computer control is integrated with an
Using Tormach PCNC 1100 Series 3
9-2
32397 Rev C1-2
Warranty, Specifications, Customization and Troubleshooting
operator control panel for spindle lockout, manual spindle controls, manual coolant control
and PC power control.
9.4.3
9.4.4
•
Digitizing & tool touch off port, optically isolated.
•
Coolant or accessory AC outlet. The AC outlet for coolant is automatically controlled via
M-codes while the operator console offers a convenient manual override.
•
PC or accessory AC outlets, manually controlled on the operator console.
•
Power requirements – Machine tool: 200 to 250 VAC single phase. Auxiliary: 115 VAC
coolant system and computer (USA)..
System
•
Complete RS-274 (G- & M-codes) implementation with virtually unlimited program size.
Conventional G- & M-code operations are complemented with manual mode operations,
operation wizards. Operation Wizards allow pocketing, surfacing, cutouts, drill patterns and
other standard operations to be completed without the need for addition software or manual
code writing.
•
Supported codes include: G00 [Default]Positioning (Rapid Traverse), G01 Linear
Interpolation, G02 Circular/Helical Interpolation CW, G03 Circular/Helical Interpolation
CCW, G04 Dwell , G17 [Default] Circular Move XY Plane, G18 Circular Move ZX Plane,
G19 Circular Move YZ Plane, G20 [Default] 06 Inch Input, G21 Millimeter Input, G40
[Default] Cancel Cutter Compensation, G41 Cutter Compensation Left, G42 Cutter
Compensation Right, G50, G51 Scaling, G52 Special offset, G53 Work Offset Cancel,
G54-G59 Work Offset, G74 Incremental Input I, J, K, G75 [Default] Absolute Input I, J, K,
G80 [Default] Canned Cycle Cancel, G81 Spotting Drill Cycle, G82 Speed Peck Drill
Cycle, G83 Full Retract Peck Drill Cycle, G85 Boring Cycle, G86 Boring Cycle – Spindle
Stop, G87-89 User Definable, G90 [Default] Absolute Input, G91 Incremental Input, G92
Set Program Part Zero, M00 Program Stop, M01 Optional Program Stop, M02 Program
End, M03 Spindle Clockwise , M04 Spindle Counter-clockwise, M05 Spindle stop, M06
Tool change, M07/M08 Coolant, M09 All Coolant Off.
Options
The PCNC comes preconfigured for low cost 4th axis addition. Software support, wiring,
cabinet holes and drive mount holes are all in place for an easy 4th axis addition.
A wide range of accessories such as tapping heads, probes, tool setting sensors, Power Draw
Bar and Automatic Tool Changer are available.
9.5
Maintenance
9.5.1
Foreword – Understanding Machine Design
The PCNC has been designed for user maintenance, but an important prerequisite to effective
maintenance is an understanding of some general machine design concepts. For many owners
the PCNC is their first experience with a serious machine tool and they may be unfamiliar with
the ideas presented here. This section should be read and understood before attempting any
adjustments to the machine.
9.5.1.1
Machine Stiffness
Iron is a wonderful thing. In the context of the human experience, the iron and steel of your mill
seems exceptionally stiff and essentially immovable. Never the less, any physicist or material
scientist will tell you that iron is a Hookean material, meaning that it always obeys Hooks Law
32397 Rev C1-2
9-3
Using Tormach PCNC 1100 Series 3
Warranty, Specifications, Customization and Troubleshooting
and will distort linearly in proportion to applied force. In simple terms, it acts like a spring.
Small force, small distortion; large force makes for a large distortion.
Precision dial indicators are also wonderful things. The ability of a $20 indicator to show
motion of a distance 0.0002” is amazing. This sort of distance is outside the scope of normal
human experience. In the context of a dial indicator, the iron and steel of your mill no longer
seems rigid. The motion of the frame under force becomes quite apparent. You should know
that this flexibility is natural. You would see more flex on an 800 lb machine and less on an
8000 lb machine. One of the keys to creating accurate parts with your mill is developing an
awareness of machine flex. The flexure of the machine and the cutting tool are the principle
reasons that a light finishing cut yields a more accurate part. There are, of course, many other
implications that flex has in planning your machining processes such as the direction of cutting
(climb versus conventional milling), tool geometry, and much more.
9.5.1.2
Backlash, Friction, and Lost Motion
All machines will show backlash. Conventional backlash is the result of open spaces between
moving parts. For example most ball bearings have clearance between the balls and races which
results in backlash. Preloading bearings is the technique of putting opposing pairs of bearings in
compression. This technique will eliminate the open space, but apparent backlash, more
correctly called lost motion, will still exist. There will always be some force required for
motion. Since the bearings are compressible (remember steel is a spring), there will be some
motion required for compression before enough force is delivered and motion is obtained. This
is lost motion and has the same effect as conventional backlash.
When you’re working to tune a machine you should be aware that if there is backlash of more
than 0.003” there is some conventional backlash and something needs to be adjusted or
replaced. Backlash of 0.0015” or less is probably lost motion and not conventional backlash.
There are compromises and tradeoffs made when you tune a machine. Tightening the gibs on
the X axis will reduce backlash in Y, but it also increases the force required for motion in X,
thus increasing lost motion in X. Increasing the preload on a bearing pair will reduce lost
motion, but it will shorten the life of the bearing.
9.5.1.3
Factors Combine
Machine setup and tuning is done under no-load conditions. The accuracy of machined work is
going to be worse because tool flex, work piece flex, fixture flex, and other factors combine
with the basic machine accuracy. Even thermal expansion adds to the mix. A 30” ball screw
will change 0.0025” in length with a 10 degree F change in temperature.
9.5.1.4
Adjusting Geometry
It’s not unheard of for a machine to need adjustment. All of the iron castings of your machine
undergo thermal stress reliving. Major elements, such as the column and base, also undergo a
vibratory stress relief process between rough machining and final machining. Never the less, it
is possible that any iron casting can change shape a small amount, whether due to changes in
the crystalline structure over time or changes induced through tool crashes and abuse.
Before making any adjustment, think carefully about the need for the adjustment and
implications associated with it. As an example, consider the G6 test on your machine QC
specification sheet. This is simply mounting a dial indicator on the spindle, about 4” from the
spindle center, then measuring the variation in distance to the table. This is sometimes referred
to as swinging the head or tramming. It’s an easy test to take, but people often overrate the
resulting measurements. If there is 0.003” difference, that’s 0.003” in 8”, or 0.00035” per inch.
This will put your milling out of square such that, with a 3/8” end mill, the flat bottom will be
off by 0.00014” and the sidewall on a 1” thick piece will be slanted by 0.00035”. The errors
introduced by tool flex and other issues will be far larger so, for most applications, the error is
acceptable and does not need correction.
Using Tormach PCNC 1100 Series 3
9-4
32397 Rev C1-2
Warranty, Specifications, Customization and Troubleshooting
If you do decide to correct, don’t make assumptions as to where the error comes from. The
error could be a specific problem, like the spindle head leaning down because the gib in the Z
axis is too loose, or it could be the combined effect from gib adjustments, the column/base
interface, or the Z saddle/head interface. If you make an adjustment in the wrong place, you
could make matters worse. As an example, if the Z axis gib is loose and the head tilts down,
someone could easily assume that they should shim the column/base connection. This would
make the column slant back to correct for the head leaning down. Now they have the machine
running in a slight parallelogram in addition to a loose head. Accuracy in deep hole drilling will
certainly suffer.
We don’t mean to overcomplicate the issue here. Adjustments can be made and are sometimes
necessary. The point of this discussion is that you should proceed slowly and think carefully,
assessing the need for any adjustment and the best method for making that adjustment. Drawing
out the machine on a piece of paper while thinking about how to do it will often make the
process clear.
9.5.1.5
Achieving Accuracy in Machining
The key to achieving maximum accuracy is understanding and controlling the magnitude and
direction of forces. Maximum accuracy is achieved when the forces are minimized, as occurs in
a finishing cut. Maximum repeatability is achieved when the forces are repeatable, both in
magnitude and direction.
Machining is a mix of science, skill, and art. The caveat in stating accuracy and repeatability is
that these factors depend on the techniques used by the machinist. A skilled machinist can often
deliver accuracy that exceeds the accuracy specified by the machine builder, while an
inexperienced machinist may have difficulty delivering the expected accuracy. With this
understanding, we cannot tell you what accuracy you will be able to achieve in your own work.
9.5.2
Protecting from Rust
Exposed iron and steel surfaces should always be protected from rust and corrosive
environments. If your machine will be unused for more than a couple days you should mist the
machine with light water repellant oil such as WD-40.
The rust preventative characteristics of coolant may not be effective in trapped areas. It is
desirable to apply way oil or machine oil directly to the table surface under the trapped area
when you mount a vise or fixture on the machine. Neglect this and you may be welcomed by a
rusty machine surface when you remove the fixture some days later.
9.5.3
Gibs, Dovetail Slideways and Lubrication
The X, Y, and Z slideways have a bonded layer of skived plastic compound, a composition of
acetyl and PTFE. The material is commonly known under the trade names of Turcite® or
Rulon®. This is state of the art technology for oil lubricated slideways and superior to plain
ground surfaces or hardened & chromed surfaces. We don’t have data on how long the material
will last on the PCNC, but we do know that there have been no reports of appreciable wear,
even on machines that are reported to have seen more than 5000 hours of operation. If you use
the oil lubrication system and keep the protective bellows in good shape, the slideways are not
normally maintenance items.
The central lubrication pump should be filled with quality way oil. This could be Perkins
Perlube WL-68, Tonna 68 (Shell), Vactra No. 2 (Mobil), Way-lube 68 (Sunoco), WayLube 68
(Texaco), Febis 68 (Esso) or equivalent oil.
A shot of lubrication should be given for each 4 hours of operation and after the machine has
stood unused for more than 48 hours.
Always make certain that the lubrication oil is clean. The oil is delivered to 15 points
throughout the machine. This includes the 12 sliding surfaces (4 each on the 3 axes) and 3
32397 Rev C1-2
9-5
Using Tormach PCNC 1100 Series 3
Warranty, Specifications, Customization and Troubleshooting
ballscrew nuts. These are some of the most critical and expensive mechanical parts of the
machine. Any dirt or foreign material suspended in the oil is going to be delivered directly to
these parts and can dramatically shorten the effective life of the machine.
Be sure to clean off the cover and surrounding area before refilling the oil reservoir. The
strainer at the top of the reservoir is only a screen; it is not a filter.
Note:
9.5.4
•
The pump is spring loaded, where the spring force creates a very light hydraulic
pressure. You can get the oil out quicker by pushing a bit, but apply too much force and
you can pop off one of the oil lines.
•
You will have a more uniform distribution of oil if the machine is moving when the
hydraulic pressure is applied.
•
The pump sucks up oil from the reservoir on the pull stroke and delivers it to the
machine on the push stroke. If at some point the oil pump seems much easier on the
push stroke then make certain that you do not have a broken oil line.
•
Extreme axis positions can expose the oil distribution channels that are cut into the way
support saddle surfaces. If the pump is used in those positions the hydraulic force of the
oil will not apply it throughout the machine as intended. Instead the oil will simply
squirt out at the point where the oil channel is exposed.
•
After a long period of inactivity or in cold conditions the oil system may become
clogged. See SB0031 – Flushing the Lubrication System in the Event of a Clog.
Way Covers
Way covers are important to keep abrasive debris out of the slide ways. Inspect the way covers
frequently and replace as necessary. Tormach stocks replacement way cover.
9.5.5
Axis Gib Adjustment
The slide ways are hand scraped as part of the manufacturing process. This means that the Z
axis saddle is fitted to the column. They are scraped in as a set and neither the saddle nor the
column can be had as a replacement component. Likewise, the base, XY saddle, and machine
table are scraped in as a set.
The slide ways have tapered gib plates (also hand scraped), where the position of the Gib Plate
controls the tightness and friction in a slide way. For example in figure 9.1b, the Y-axis Gib
Plate is part of the Saddle and is held in position on both front and back via the Gib Screws (see
cutaway in figure 9.1b).
Adjustment Procedure:
The adjustment procedure is similar for all
three axes. The Z axis is described in detail.
The Gib Plate is tapered down. When the Gib
Plate is moved down relative to the Z-axis
Saddle the slide way will become tighter, when
it moves up the slide way will become looser.
With the machine is turned on, move the Z-axis
up to near the top of its travel. Remove the
screws that attach the way cover to the Z-axis
Saddle in order to gain access to the lower Gib
Screw.
Figure 9.1a – Upper Z gib screw
It is difficult to assess the correct clearance for the Gib as a very small force on its end can, via
the shallow taper, apply a large force to the dovetail. Too tight a gib results in zero gap and very
Using Tormach PCNC 1100 Series 3
9-6
32397 Rev C1-2
Warranty, Specifications, Customization and Troubleshooting
high friction since there is no longer space for an oil film. The easiest method is by a form of
Figure 9.1b – Typical arrangement of gibs and screws for X/Y slide
"dead reckoning". First make sure the Lower Gib Screw is loose by a few turns (this allows
clearance for the Gib to be adjusted downward), then tighten the Upper Gib Screw in, thus
pushing the Gib down until it is tight yet not hitting the bottom screw. Wiggle the head while
you are tightening this screw to get the gib reasonably tight (this means "tight" but not so tight
you are stripping the screw head or flexing the castings... ). Next, loosen the Upper Screw 4
full turns. Now tighten the Lower Screw thus pushing the gib back up against the upper screw
(and creating a positive amount of "Gib Clearance"). Now the gib should be held in place with
the upper and lower screw tight on the gib.
Note: it is important that after any gib adjustment that both adjustment screws are tight. Failure
to do this will result in the gib moving, and all your hard work going for nothing.
A more precise method of adjusting the gibs is to use lost motion (apparent as backlash on a
dial indicator) to arrive at the correct setting. First, loosen the Upper Screw 8 turns and tighten
the Lower Screw 8 turns so that the
Gib Clearance is quite loose. Use a
dial indicator to measure the axis
backlash. With a very loose gib,
the measured backlash is entirely
attributable to the backlash in the
angular contact bearings and the
ball nut. On a newer machine the
value should be under 0.0014” on
the Z axis (note: under .001" on X
and Y). Next, tighten the Gib by
one turn (by loosening the Lower
Screw first, then tightening the
Upper Screw). Measure the
backlash again. Repeat this
procedure until the measured
backlash increases – this is the point
Figure 9.1c – Changes in backlash with gib tightness
32397 Rev C1-2
9-7
Using Tormach PCNC 1100 Series 3
Warranty, Specifications, Customization and Troubleshooting
at which the gib setting has started to induce lost motion in the axis. Back the adjustment off to
the point just before you saw the increased backlash. That is the ideal setting for the axis (see
figure 9.1c).
For the X axis, the Gib tightens with the Gib Screw on the left. No covers need to be removed.
For the Y axis, the Gib tightens with the Front Gib Screw. The front and rear Y-way bellows
need to be removed where they screw to the Saddle.
9.5.6
Adjusting Ballscrew Preload
The ball screw itself is of the double-nut preloaded design. The preload is set at the factory via
a precision ground spacer placed between the two ball nuts. They are not user adjustable. Under
typical conditions there is less than 0.0004” of lost motion attributable to the ball nut.
Figure 9.2a – Section view of X-axis mount
The ball screw mount bearings
are at the motor end of the ball
screws. These are preloaded
angular contact bearings and are
user adjustable. They are
typically adjusted for 0.0003” to
0.0013” of lost motion. Bearings
are available individually and
two are needed for each ball
screw.
If the Bearing Adjustment Nuts
are not set properly then there
will be either excessive backlash
in the machine (too loose) or
rapid wear and excessive friction
Using Tormach PCNC 1100 Series 3
Figure 9.2b – Photograph of X-axis mount
9-8
32397 Rev C1-2
Warranty, Specifications, Customization and Troubleshooting
(too tight). Figure 9.1 shows the X-axis bearings, ballscrew and motor. The Y-axis and Z-axis
are similar.
The recommended procedure for checking backlash is to observe motion at the table or head
(via a dial indicator) while moving the machine using the axis motors. Tormach recommends
adjusting the backlash on X and Y to something between 0.0004" and 0.001". The
recommended backlash for Z-axis is 0.0006" to 0.001".
Checking backlash by pushing or pulling on the axis is a less accurate method. The push/pull
method will normally show a smaller backlash value. You can fool yourself into thinking there
is zero backlash when the effective lost motion is within specification.
9.5.6.1
Understanding Preloaded Angular Contact Bearings
Figure 9.3 – Detail of bearing system
Figure 9.3 shows a cross section of a typical ball screw shaft mount. The ball screw shaft is in
the center and the crosshatched section is the iron
casting that mounts the bearings. There are two
angular contact ball bearings, forming a preloaded
pair. The cover plate holds the two outer races
together, along with the spacer that is between them.
The inner races are held between the sleeve (left side)
and the shoulder cut into the ball screw shaft. The
sleeve is held against the left inner bearing race by
the adjustment nut and a locknut; as the adjustment
nut is screwed toward the bearing pair, the preload
increases.
Figure 9.4 – Angular contact bearing
Figure 9.4 shows how the force of preload is
transmitted through the bearings, from the inner race
to the outer race. In a preload pair, this force is then
transmitted back to the inner race by an opposed
bearing. It should be apparent that the correct
orientation of the angular contact bearing is critical to
the operation.
9.5.6.2
Making the Adjustment
In order to make the adjustment you will need two
hook spanner wrenches (PN 30485) in order to rotate
the two nuts on the ballscrew end (figure 9.5).
32397 Rev C1-2
9-9
Figure 9.5 – Spanner wrenches
Using Tormach PCNC 1100 Series 3
Warranty, Specifications, Customization and Troubleshooting
The nut nearer the bearing housing is the adjustment nut and the one nearer the stepper motor is
the lock nut.
When working on the Z-axis you should remove any tooling from the spindle and support the
head by resting the spindle
nose on a block of lumber.
Loosen the lock nut and
back it off about two turns.
Hold the ballscrew to
prevent it from rotating
with a pair of pliers on the
coupling and tighten the
adjustment nut until there
is slightly more backlash
than you ultimately want to
achieve – tightening the
lock nut will slightly
increase the bearing
preload.
Figure 9.6 – Feeling preload in bearings
There are two possible
methods to judge the preload:
(a) You can use a dial test
indicator to measure
backlash between the
ballscrew end and the
structure to which the
bearings are mounted
(table for X-axis or
machine frame for Yand Z-axes);
(b) You can estimate the
torque required to turn
the ballscrew in the
bearings.
If you are aiming for the smallest
possible backlash then we suggest
that you do both as it is not possible
to be certain that you do not have
excessive preload by just measuring
backlash.
Figure 9.7 – Tightening the lock nut
To estimate bearing drag torque you
need to eliminate the stepper detent torque and the ballnut friction. This is done by allowing the
stepper mounting box to rotate and measuring the torque
required to do this.
(a) For adjusting the X-axis position the table near the right
hand end of its travel (i.e., X near to zero). This ensures
that the bearing is near to the ballnut to minimize
bending of the screw during tests.
(b) Slacken the two screws clamping the coupling between
the stepper shaft and ballscrew end.
(c) Remove the four cap screws holding the stepper motor
to the coupler box. Remove the stepper. This is the
Using Tormach PCNC 1100 Series 3
9-10
Figure 9.8 – Another view of
tightening the lock nut
32397 Rev C1-2
Warranty, Specifications, Customization and Troubleshooting
reverse of the process for coupling the Y-axis drive shown in section 2.3.
(d) Remove the four cap screws holding the motor coupler box to the table (X-axis) or frame of
the machine (Y- and Z-axis). Move the axis so the mounting box comes free of its pins. The
screw and box are supported on the ballnut so take care not to apply forces that could bend
the screw (figure 9.6).
(e) You can now rotate the box by hand and get a sensitive feel for the torque caused by the
preload on the bearings. Rotation should be smooth with a small perceptible drag this
corresponds to a medium preload of about 150 lbs. If the rotation feels tight you have too
much preload and will dramatically shorten the life of the bearings. If the rotation is free
and/or the box can be rocked perpendicular to the screw axis then you have little on no
preload and backlash will be excessive. This test should be done with the lock nut tight. It
is best to support the box on its dowel pins when adjusting the nuts to avoid damaging the
ballnut or risking bending the screw.
(f) Finally remount the box and motor ensuring that the coupling is symmetrically fitted to the
motor shaft and the screw end and is fully tightened (figure 9.7 & 9.8).
9.5.7
Adjusting Mating Surfaces
The mating surfaces between components are pinned with tapered metric dowels. The dowel
holes are drilled after the parts have been aligned. The pins help maintain alignment during a
tool crash and allow restoration of original alignment in case the parts have to be disassembled.
Alignment between components can be adjusted with shims. In most cases any adjustment will
only require a few thousandths of an inch and will not require a full disassembly. Normally the
bolts can be loosened, the alignment dowels left in place, and the shim stock inserted in a small
opening. Often the machine motion can be used to open the space to insert the shim stock. If
alignment needs to be changed and requires removal of a dowel pin, the recommended
procedure is to over drill and ream for the next large size dowel pin after adjustment. Each
dowel pin has a small metric threaded hole in the center that can be used to extract a dowel.
9.5.8
Speed Calibration
This procedure is not necessary for operation of a machine, it is only recommended as an
improvement to spindle speed accuracy. The spindle speed in your PCNC is factory calibrated,
but your computer is not calibrated to your machine. The variations among PCs will affect the
precision of the computer generated spindle speed. To improve spindle speed accuracy, your
computer needs to be calibrated to your PCNC.
The PCNC uses a printer port of a standard PC for its machine control. The procedure described
below will calibrate the PCNC to a specific computer. The procedure should be repeated any
time the machine control computer is replaced.
While the there is no electrical work involved, the procedure does require access to the
electrical cabinet while under power. Points within
the cabinet will contain high voltage. Exercise caution
whenever opening the cabinet if the machine is under
power.
1. Turn on the machine and control computer and
then open the PCNC control software program.
2. Set the belt to the LOW speed range and set the S
word to 500 either by MDI of S500 or typing the
value into the S DRO followed by Enter.
3. Start the spindle.
4. Inspect the value displayed on the panel of the
VFD. It should be around 35 Hz. See figure 9.9
32397 Rev C1-2
9-11
Figure 9.9 – VFD frequency readout
Using Tormach PCNC 1100 Series 3
Warranty, Specifications, Customization and Troubleshooting
(this photo was shot with the
machine running near top speed)
Record the frequency shown.
Shut down the PCNC Control
Software.
5. Open the PCNCConfig software
program located under
“Programs” on your “Start”
menu. This will have been
installed when you installed the
control software. Click the “Open
Profile” button and choose the
machine profile you wish to
modify (figure 9.10). The profile
for the PCNC 1100 is:
C:\PCNC3\PCNC1100M33.xml.
Figure 9.10 – Opening the profile
6. Next, under the “Speed Calibration” heading enter the frequency you recorded earlier
(figure 9.11). The software will display a new "Spindle steps per unit" value.
7. At this point, you should click the “Save Profile” button. If you are sure all the information
is correct, click the “Done” button. Close the PCNCConfig software program.
8. Open the PCNC control software program again and confirm that the computer is calibrated
with the machine by repeating step
4 and checking that the frequency
is 34.6 Hz.
9. Occasionally, repeating the above
steps may be required to hone in
on the target speed.
Note:
Since each computer is different, it is
important to re-run the PCNCConfig
program whenever you connect a new
computer to your PCNC.
.
Figure 9.11 – The measured frequency
Using Tormach PCNC 1100 Series 3
9-12
32397 Rev C1-2
Warranty, Specifications, Customization and Troubleshooting
Figure 9.12 – Finding printer port
9.5.9
Using a Non-standard Printer Port
There are several reasons why you may wish to use a different printer (parallel) port from the
one on your PC’s motherboard – for example a PCI bus plug-in card. In this case you will
almost certainly need to reconfigure the PCNC Control Software to use a different address from
the standard motherboard address which (in hexadecimal) is 0x378.
Use this procedure.
1. Close the Control Software if you have it open.
2. Click on the Start Menu and choose Control Panel
3. On the top left-hand side, click on Switch to Classic View. Note: If it says “Switch to
Category View” that means you have already switched to “Classic View.”
4. Double click the System icon.
5. Choose the “Hardware” tab and click on “Device Manager.”
6. Find the “Ports (COM & LPT)” icon and click on the plus sign (figure 9.12 shows the
result of these steps).
7. Double click on “ECP Printer Port (LPT1)” – wording may differ depending on your
system. If you are looking for a plug-in card then the card name will probably appear in
the title.
32397 Rev C1-2
9-13
Using Tormach PCNC 1100 Series 3
Warranty, Specifications, Customization and Troubleshooting
Figure 9.13 – IO address in Resources
Figure 9.14 – Entering port address
8. Choose the “Resources” tab and take note of the first number under “Setting” that
corresponds with the first “Resource Type” I/O Range (figure 9.13). This shows the
standard value for a
motherboard port. A PCI
post will not start with a
zero – it will probably be
something like CD80 (as
it is a hexadecimal
number it can have digits
A, B, C, D, E or F in it).
Write down the four
numbers and/or letters.
This is your “Printer port
address in Hex.”
9. Finally, run the
PCNCConfig program
and open the PCNC3
profile (details in section
9.5.8 above) and enter
this number under the
“Printer Port” heading
(figure 9.14).
Figure 9.15 – Step sizes in PCNCConfig
9.5.10 Defining Your Own Sizes for Step-mode Jogging
When Step jogging (either by keyboard or the Jog/Shuttle controller) the size of step that will
be take is in the Step DRO. You can put any value you like into here. For safety avoid large
movements.
The control software has a table of standard increments and you can go through these one by
one and put them into the Step DRO using the Jog Step button.
The values in this list can be configured using PCNCConfig.
Using Tormach PCNC 1100 Series 3
9-14
32397 Rev C1-2
Warranty, Specifications, Customization and Troubleshooting
You can either setup your own sequence in the indicated boxes or use a sequence of two small
steps. Buttons are provided for metric steps (2 microns and 20 microns) or imperial steps
(0.0001" and 0.001")
If you choose your own steps you should take care that there is no unexpected jump going from
the end of the list to the start.
9.5.11 Defining Probe Type
The accessory port on the user panel can be used as an input port for a digitizing probe.
The Tormach Probe closes a contact when a touch is made and consequently is the default
setting in the Probe Logic Sense portion of the PCNCConfig program.
A number of aftermarket probes require the opposite logic for proper function (opens a contact
on touch). If an aftermarket probe of this sort is to be used, change the Probe Logic Sense using
the indicated pull down menu (figure 9.15). Please note that it is up to the user to ensure that
proper wiring and source voltages are recognized. Please refer to section 8.2.4 for more
information.
9.5.12 Enabling 4th axis homing
To enable the optional 4th axis homing kit, please refer to figure 9.15 and select "Homing
Enabled.
9.5.13 Configuring to start in Metric units
The PCNC is designed based on the imperial (inch) system of units. Thus one step of each axis
is exactly 0.0001". It is, however, equally capable of working in metric units. The only
limitation you will encounter is that if you look at the raw tool and work offset tables you will
see that they are always in inches. Everything else on the screens is automatically in the units
you have currently got selected.
In order to startup the system in metric each time you need to edit the file:
C:\PCNC3\macros\PCNC-M3\m990.m1s
The start of this file looks similar to this:
' This macro implements PCNC INIT actions
' Add G21/G20 change if needed
' Uses UserLabel 2, UserDRO 1209
Using a simple text editor (e.g. Notepad++) add the following line after this code
Code "G21"
' make PCNC to start in metric (i.e. G21 mode)
Save the edit. The machine will then start in G21 (metric) mode.
32397 Rev C1-2
9-15
Using Tormach PCNC 1100 Series 3
Warranty, Specifications, Customization and Troubleshooting
9.6
Troubleshooting
9.6.1
Overview
Tormach is taking a different approach to troubleshooting documentation than is typically
encountered. We feel that a discussion of general troubleshooting methods is quite important,
yet we have not seen this information presented by others.
We have therefore begun this document with a section on the Philosophy of Troubleshooting.
We feel that if you spend a few minutes on this section, you will be in a better position to
effectively trouble shoot problems.
The Philosophy of Troubleshooting is followed by a section containing Tips and Tools for
Troubleshooting.
Next comes a list of Frequently Found Problems (FFP’s) which comes from our experience in
working with customers. We urge you to review this section every time you are having a
problem. There is a reason the items made it to this list.
The remainder of this document addresses troubleshooting in each of several subsystems on the
machine. Within this major troubleshooting section are three distinct areas:
•
An overview of the Sub-system
•
A Problem Resolution Checklist
•
A Detailed Description of the Electrical Circuit
A detailed description of each subsystem is provided for users who want in-depth knowledge of
the machine and who would prefer to take that knowledge and apply it to troubleshooting rather
than to follow a checklist. For those who prefer to follow a step by step procedure, the Problem
Resolution Checklist is provided.
Figure 9.16 is flowchart showing the recommended order in which to use the sections of this
troubleshooting section of the manual.
9.6.2
Philosophy of Troubleshooting
The PCNC1100, like many modern machines, is an integration of mechanical components,
electrical components, a computer, and software. Taken as a whole, the PCNC is a
sophisticated machine; however, the machine is comprised of several sub-systems, each of
which is much easier to understand than is the machine in its entirety. That, in fact, is the first
key principle in troubleshooting, sometimes referred to as the “Divide and Conquer” approach.
It is working on one problem at a time, and focusing on only those things that can be related to
the problem.
So what is the second key principle in step in troubleshooting? Simply put, it is an
understanding of how the machine is supposed to work. It is not possible to know that a
machine is functioning improperly if one does not know how the machine is supposed to
behave.
The third key principle in troubleshooting is noting what has changed in the environment since
the machine worked properly. This principle becomes a larger factor after the machine has been
in service for some time because the start-up learning process is complete and any “kinks” with
the hardware have been worked out. The following are some events which could cause
difficulties.
•
The machine was moved
•
There was a thunderstorm and lots of lightning since the machine was last used and now
the electronics don’t work
•
There was water in my basement where the machine is located
Using Tormach PCNC 1100 Series 3
9-16
32397 Rev C1-2
Warranty, Specifications, Customization and Troubleshooting
•
It froze hard last night and the machine is in my unheated outbuilding
•
My son was home on spring break and he may have run the machine while I was away,
or even did something with the computer.
•
There were problems when I tried to cut steel. I had only cut aluminum and plastic prior
to this.
A fourth key principle is to work smart. One should always make a list of tests which can be
done (make sure to save room for recording your results). After making up the list, rank the
tests in order of difficulty in performing the test. Then, do the simple tests first and then do the
tests that seem to address the most likely cause of the problem. We will rank the probability of
the various potential causes of problems. We will also make note of those problems we have
found to be FFP’s (Frequently Found Problems).
A fifth key principle is to complete one test before starting anther. Don’t fall victim to making
things worse by troubleshooting. More than once a troubleshooter has removed a wire to make
a measurement and in his haste to solve the problem, moved on to the next test without putting
the wire back on. This can impact the next test and certainly will impact the machine operation.
32397 Rev C1-2
9-17
Using Tormach PCNC 1100 Series 3
Warranty, Specifications, Customization and Troubleshooting
Philosophy
Tips and Tools for
Troubleshooting
Frequently Found
Problems
Find Appropriate
Sub-System
Read Subsystem
Overview
Do you find yourself
needing an electrical
schematic to troubleshoot or
would you like to be able
to use one when
troubleshooting?
Yes
Proceed to the
Details Section in
the Relevant
Sub-section
No
Apply your
knowledge and try
to solve the
problem
No
Is your problem
solved?
Proceed to
Problem
Resolution
Checklist in the
Relevant
Sub-Section
Is your problem
solved?
Yes
Yes
Congratulations,
Well done
No
Call Tormach
Technical Support
Figure 9.16 – Troubleshooting overview
We will build on these key principles by providing a description of each of the sub-systems on
the PCNC. This will serve to help the user understand how the machine should work and
provide an overview of the components that are involved in the sub-system. We will also list
some guidelines for equipment and procedures used in troubleshooting.
Using Tormach PCNC 1100 Series 3
9-18
32397 Rev C1-2
Warranty, Specifications, Customization and Troubleshooting
As in most electromechanical machines, it is frequently easier to see problems in the
mechanical systems than the electrical and computer systems. With this in mind, most of the
details in the troubleshooting section will address non-mechanical areas.
The user may find that this background information will allow him to troubleshoot without any
assistance from Tormach. At the minimum it should allow the user to begin the process of
troubleshooting and make any contact with Tormach Technical Support go more smoothly.
Review of the Key Principles for Troubleshooting
• Know how the machine is supposed to work
•
Divide and Conquer—focus on one area
•
Analyze what has changed
•
Work Smart — do the easy and obvious tests first
•
Complete one test before starting another.
9.6.3
Tips and Tools for Troubleshooting (Equipment and Procedures)
9.6.3.1
Safety
Safety is always important. During troubleshooting one tends to expose themselves to more
hazards than they incur during normal operation. Electrical tests may have to be done to live
circuits. Guards may have to be removed and sometimes a safety switch will have to be
“fooled” in order to make an observation. Take things slow and be extra cautious.
Keep in mind that we are not going to repeat a big safety paragraph before or between every
step of a troubleshooting procedure. Doing so tends to underscore its importance. But do
yourself a favor and think about safety whenever you are taking any action.
9.6.3.2
•
Never do anything with machine power on that can be done with machine power off.
•
Wear eye protection and use appropriate protective clothing such as gloves
•
Don’t wear loose clothing
•
Don’t wear jewellery
•
Don’t do any electric testing if the floor is wet. Don’t run the machine either.
•
Don’t put your hands anywhere you don’t have to. Keep your hands in your pockets if
you can.
•
Think about each move you are going to make and what you can do to be as safe as
possible before making the move.
•
Focus on the task alone. If you feel preoccupied with something else and you think your
mind could be wandering, wait until such time as you can concentrate fully on the task.
Tip on Computer Diagnostics
The Control Software provides a diagnostic screen which can be useful for troubleshooting.
Become familiar with this screen.
The software also has an information line next to the “Reset” that can provide valuable
information.
If calling Tormach Technical Assistance, make sure you know what version number of
software, machine profile and screen you are running and have recorded information from the
diagnostic screen and the "error" line.
32397 Rev C1-2
9-19
Using Tormach PCNC 1100 Series 3
Warranty, Specifications, Customization and Troubleshooting
Figure 9.17 – Location of version numbers
9.6.3.3
Tools
The following are the minimum tools one should have on hand for troubleshooting
9.6.3.4
•
Good lighting so you can truly see what you are looking for: a trouble light or a
headlamp or a flashlight
•
A digital multi-meter that can test for AC volts, up to 300 V, DC volts, up to 100V and
Resistance, from 0 to 1MΩ (Ω is the common symbol for ohms)
•
Assorted screwdrivers: #2 and if possible a #3 Phillips, 1/8" and 3/16" flat blade
•
A wire stripper
•
Measuring tools: Tape measure, Calipers, Dial Indicator (Optional)
Using the digital multi meter for electrical tests
Almost all Digital Multi-meters have the capability of measuring AC Volts, DC Volts, and
Resistance. These are the important functions use when troubleshooting a Tormach PCNC.
Two test leads are required to measure these three functions. While many meters have more
than 2 receptacles in which to plug leads, for our purposes the leads will always remain in the
same 2 receptacles. One receptacle is almost universally labeled COM (for Common) and the
black lead is to be plugged into this receptacle. The other lead, most often red in color, is
plugged into the receptacle labeled VΩ (for volts and ohms).
Measuring DC voltage
Select the DC voltage scale on the meter. The scale may be labeled DCV or
DC voltage has polarity so if the common lead on the meter is not placed on the common
signal, the voltage will read as a negative number. This will not harm the meter, but could be
confusing in certain cases. We will strive to define the common terminal when asking you to
take a measurement.
Measuring AC voltage
Select the AC voltage scale on the meter. The scale may be labeled ACV or
There is no polarity to AC voltage so either lead can be placed on either location we are having
you measure.
Using Tormach PCNC 1100 Series 3
9-20
32397 Rev C1-2
Warranty, Specifications, Customization and Troubleshooting
Measuring Resistance (Ω is the symbol for ohms which are the units in which resistance is
measured)
Select the resistance scale on the meter, most often labeled Ω.
There is no polarity to resistance so either lead can be placed on either location we are having
you measure; however, resistance measurements are always taken with power off.
Note: When making resistance measurements on motors and other devices with low resistance,
always take a tare* or zero reading on the meter before doing the resistance measurement on
the motor or device.
*A tare reading is a reading using only the instrument. In the case of using a digital multi-meter
to measure resistance, touch the probes together to get the tare reading. Subtract the tare reading
from the meter reading when measuring the resistance of the motor to get a true value.
9.6.3.5
Contacting Technical Support
[email protected]
608-849-8381
There will be times when your troubleshooting efforts don’t end up solving a problem. There
are a number of things that will make problem resolution easier should your be required to
contact Tormach Technical Support.
1) Always have the serial number of your machine.
2) Tell Tormach if you have had the problem before. Tormach uses a case management
system for tracking problems. If you contacted us in the past with a problem, you should
have a case management number which will be helpful to us.
3) Tell us if you bought the machine from someone else and have the name of the party
available so that we can consult our case management system for problems that may have
occurred on the machine for the previous owner.
4) Analyze what might have changed since the machine worked properly.
5) Read over the description of the subsystem involved to improve your understanding of that
subsystem.
6) Make sure you can repeat the problems. Do it a few times and record the results. Determine
if you can repeat the problem exactly.
7) Record information from the diagnostic screen of the control software
8) Try to define the problem as concisely as possible. Most often it is a good idea to write
down the problem definition. Many times when doing this you find it leads you to
answering the problem yourself.
9) Consider sending Technical Support an email rather than calling if time permits. It is often
best to send an email rather than call because it tends to force you to define the problem
better. When you correspond by email you don’t have to worry about keeping notes or
having to interpret the hastily transcribed notes one takes during a phone conversation.
Even if you want to call, having first sent an email can help the conversation go better.
9.6.4
Frequently Found Problems (Repeat Offenders)
There are several frequently found problems with all electro-mechanical machinery such as the
Tormach PCNC. It is not that the problems are frequent, but among the problems that have
occurred, these are more frequent than others.
The first 6 items in this list fall into the category of machinery in general, while the last items
are specific to the PCNC. These repeat offenders are important to keep in mind when
troubleshooting.
9.6.4.1
Loose Wires
Try as we might it seems that on occasion we find a poor wire connection. This can be the wire
in a screw clamp terminal where the clamp is loose, a problem with a crimp spade or ring
32397 Rev C1-2
9-21
Using Tormach PCNC 1100 Series 3
Warranty, Specifications, Customization and Troubleshooting
connector where the connector is tight in the screw clamp terminal but the wire is loose in the
crimp connector. This is most frequently found during the initial startup of the machine. The
vibration that occurs during ravel tends to loosen connections. Use the 2 finger pull test--grasp
the wire close to its termination point between your thumb and index finger, and gently but
firmly tug each wire. If the wire comes loose, re-terminate it before moving on to other wires.
One of the graybeards at Tormach recalls industrial customers in the paper industry who were
so plagued by problems caused by poor connections that they shut their entire operation down
for days and checked virtually all connections. This act solved many problems for them.
9.6.4.2
Wire Hairs
Sometimes with stranded wire we find that a “wire hair” from the stripped end of the wire may
be sticking out from the wire and touching another wire or the machine frame. This can cause
short circuits.
9.6.4.3
Poor Cable Connections
There are a number of cables on a PCNC. Some are flat cables connecting the Tormach Control
Board to the Axis Drives and other devices and some cables connect with the computer. An
improperly seated cable can allow some functions to work and others to not work. We have
found that the ribbon cables plug connections can become loose during the shipping process.
9.6.4.4
Software Restart
It is rare but not impossible that the application software can get confused (imagine that). If an
unexplained problem is occurring it may be worthwhile to restart the application (in the case of
the PCNC, it is the Mach3 software). It is usually not required to restart the computer, but being
a relatively easy thing to do, it should be considered.
9.6.4.5
Sensors (on the PCNC the End of Travel Sensors)
Sensors are one of the largest causes of problems with any machine. On the PCNC, the X and Y
Axes have 1 limit switch which actuates at the end of travel in each direction of both axes. The
Z axis on earlier machines has 2 limit switches, one for up and one for down. Newer machines
have one for the up direction. These sensors will be discussed at length in the Axis
Troubleshooting section of the manual.
9.6.4.6
Flaky Computer
Computers can exhibit some intermittent problems. A number of Tormach customers have
purchased used computers for a song but ended up singing the blues. Remember the computer
you bought on E-Bay or the like were probably being sold for a reason. Lots of unexplainable
problems have been cured by swapping out computers whose history was unknown. It is far
better to put an old computer you have confidence in on your machine than take a chance on an
unknown used computer. Used computers have been found to be more susceptible to electrical
noise.
Laptop computers will almost never work on a PCNC and should not be considered.
9.6.4.7
Control Software license not installed
The control software can be installed without the license. It will run small programs without the
license being activated. Once a program exceeds approximately 500 lines, the program will fail
to execute the following line and the program will halt without warning. No other diagnostic
information will be displayed. Machine Controllers purchased through Tormach will have the
control software loaded, but WILL NOT have the license loaded. It is up to the user to load the
license CD that came with the machine.
Using Tormach PCNC 1100 Series 3
9-22
32397 Rev C1-2
Warranty, Specifications, Customization and Troubleshooting
9.6.4.8
Unexplained stop or limit switch error while running
Electrical noise can cause “strange and un-repeatable” problems. Tormach has found that by
adding a Ferrite suppressor to the Parallel Port Cable going from the computer to the machine
will eliminate many of these problems. We have also found that simply adding a second
Parallel Port Cable in series with the existing cable reduces the problems with electrical noise
If extension cables are used frequently there are exposed metal parts on the connectors. If these
metal parts contact other metal objects such as the machine frame, noise problems have been
observed. Taping off the exposed metal parts of the connectors to prevent contact has proven to
be effective.
9.6.5
Which sub-system should I troubleshoot
32397 Rev C1-2
9-23
Using Tormach PCNC 1100 Series 3
Warranty, Specifications, Customization and Troubleshooting
Start
Is there any electrical
power on the machine?
Proceed to the
Power Distribution
Sub-section
No
Yes
Can you turn on Control
Power (Machine LED is
on)?
Proceed to the
Control Power
Sub-section
No
Yes
No
Proceed to the
Computer Control
Sub-Section
Can you turn on the
computer LED?
Yes
Are the X,Y,Z, and A Axes
Function Properly?
Proceed to the
Axis Drive
Sub-section
No
Yes
Is the Spindle Drive
Functioning Properly?
Proceed to the
Spindle Drive
Sub-section
No
Yes
End
Figure 9.18 – Deciding which sub-system to troubleshoot
The flowchart in figure 9.18 will guide you where to start troubleshooting the electrical system.
9.6.5.1
Computer and Coolant Power Distribution Sub-system
Overview
User supplied electrical power is run through the disconnect switch on the machine. This switch
turns on and off all the electrical power to the entire machine and the computer system.
Using Tormach PCNC 1100 Series 3
9-24
32397 Rev C1-2
Warranty, Specifications, Customization and Troubleshooting
You will find listed immediately
below a Problem Resolution
Checklist section. For more in
depth explanation of this
subsystem, please go to the Details
section that is after the Checklist
section.
Figure 9,19 – Power Disconnect
Problem Resolution Checklist for the Power Distribution Sub-system
Contents of the Power distribution Sub-System Problem Resolution Checklist
Table 1.1
GFI in customer supply for power for the computer and coolant pump trips
Table 1.2
Computer will not power up
Table 1.3
Coolant Pump will not run when Coolant Switch is in the ON Position
Power Distribution Checklist
Table 1.1
GFI in customer supply for power for the computer and coolant pump trips
Possible Cause
ProbAction to identify Cause
Discussion
ability
of Problem
GFI circuit defective
High
Test a device such as a
If the tool works, the circuit is OK
drill or other portable tool
on the circuit
Loose wires in circuit
Medium
Remove power from the
Use the two finger tug test — see
machine by turning off the “Loose Wires” in the Frequently
disconnect switch and test Found Problem list
for loose wires
Bad Control Board
Low
Remove power from the
You can also unplug the power cord
machine by turning off the for the machine
disconnect switch
Remove wires 202 and
If the problem disappears, a Control
205 from the Tormach
Board problem is indicated. You can
Machine Control Board.
run the machine by controlling the
Tape each wire
coolant pump in Manual until your
individually so it cannot
are able to replace the Control
short out, then re-apply
Board.
power.
32397 Rev C1-2
9-25
Using Tormach PCNC 1100 Series 3
Warranty, Specifications, Customization and Troubleshooting
Possible Cause
Computer switch
(SW6) on Operator
panel turned off
Disconnect Switch in
off position
Breaker turned off in
user panel supplying
PCNC or GFI (if used)
Tripped
Computer not plugged
into outlet
Probability
High
Power Distribution Checklist
Table 1.2
Computer will not power up
Action to identify Cause
Discussion
of Problem
Check the switch
Turn it on if required
Medium
Check the switch
Turn it on if required
Medium
Check the breaker and GFI
Turn it on and/or reset if required
Medium
Check the plug
Plug it in if required
Power Distribution Checklist
Table 1.3
Coolant Pump will not run when Coolant Switch is in the ON Position
Possible Cause
ProbAction to identify Cause
Discussion
ability
of Problem
Coolant Pump not
High
Check the plug
Plug it in if required
plugged into outlet
Breaker turned off in
Medium
Check the breaker and GFI Turn it on and/or reset if required
electrical wall cabinet
supplying PCNC or
GFI (if used) Tripped
Disconnect Switch in
Low
Check the switch
Turn it on if required
off position
Using Tormach PCNC 1100 Series 3
9-26
32397 Rev C1-2
Warranty, Specifications, Customization and Troubleshooting
Figure 9.20 – Power distribution portion of schematic
Details of the Power Distribution Sub-system
The PCNC is powered by a user provided nominal 230/1/60 (230 V single phase, 60HZ) 20
Amp, 3 wire electrical circuit in North America and a 220/1/50 20 Amp, 3 wire electrical
circuit in most other parts of the world. Tormach allows the voltage range to be from 200VAC
to 250 VAC. The 2 current carrying conductors of this supply are connected to the Tormach
disconnect switch located on the right side of the electrical panel. When this disconnect switch
is in the off position, no power is applied to the main machine. Find the relevant portion of the
electrical schematic highlighted below. You may find it helpful to have your electrical
schematic available to use along with this discussion.
32397 Rev C1-2
Figure 9.21 - Machine Cabinet Component Locations for Power Distribution
9-27
Using Tormach PCNC 1100 Series 3
Warranty, Specifications, Customization and Troubleshooting
In addition to the main electrical supply to the machine, provisions are included so the user can
supply a second electrical circuit to the cabinet. This second circuit is used to provide power to
the computer and monitor and to the coolant pump. The power source for this circuit is
110/1/50, 115/1/60 or 220/1/50 single phase power with one leg of the 2 current carrying
conductors grounded. Normally, a 115 VAC circuit would be supplied in North America. A
third wire ground must also be provided. The ungrounded leg of this supply is connected to a
third pole on the disconnect switch described in the paragraph above. Running this circuit in
this manner allows the coolant pump outlet to be controlled either automatically by the machine
under computer control or manually depending on the position of the Coolant switch, SW5, on
the operator panel. The circuit also provides power to 2 outlets which can be used for the
computer and monitor. These outlets are controlled by SW6, labelled Computer, on the operator
panel. This allows turning off the computer when power is still applied to the main machine.
Turning the disconnect switch to the off position removes power to the coolant and computer
outlets.
9.6.5.2 Control Power Sub-system
Overview
Figure 9.22 - Operator Panel start, stop and machine LED functions
Control Power enables running of the machine. When Control Power is on, some components
in the cabinet are live but none of the motors and drives are powered up. Turn Control Power
on when your desire to run the machine by pressing the start PB (push button) and turn off
Control Power by pressing the stop PB when you are not running. The stop PB is a twist lock
device. The button must be released by turning the button clockwise until the button “pops out”.
The “machine” LED illuminates when Control Power is on.
You will find listed immediately below a Problem Resolution Checklist section. For more in
depth explanation of this subsystem, please go to the Details section that is after the Checklist
section.
Using Tormach PCNC 1100 Series 3
9-28
32397 Rev C1-2
Warranty, Specifications, Customization and Troubleshooting
Problem Resolution Checklist the Control Power Sub-system
Possible Cause
Stop button is in the
locked position
Breaker turned off in
electrical wall cabinet
supplying PCNC
Disconnect Switch in
off position
Control Power Sub-system Checklist
Table 2.1
Control Power Cannot be Turned On
ProbAction to identify Cause
Discussion
ability
of Problem
High
Twist the head of the
button to release
Medium
Check the breaker
Turn it on if required
Low
Check the switch
Fuse FU1 and/or FU2
blown
Low
Fuse 3 or 7 blown
Low
Transformer XFM1 bad
Low
Measure for 230 VAC
nominal between wires
L11 and L21
Measure for 115 VAC
nominal between wires
102 and 100
First ensure fuse 3 is not
blown then measure for
115 VAC nominal
between wires 102 and
100
Turn it on if required. Measure for
230 VAC nominal between wires L1
and L2 if required
Turn off Disconnect Switch before
checking or replacing fuses
Turn off Disconnect Switch before
checking or replacing fuses
Turn off Disconnect Switch before
replacing transformer
Details of the Control Power Sub-system
Find the relevant portion of the electrical schematic highlighted below. You may find it helpful
to have your electrical schematic available to use along with this discussion.
The Control Power circuit is that circuit which is energized when in a ready to run state and
which de-energizes when the red stop button (PB1) is in the depressed position. The circuit
does not energize until the Stop Pushbutton is released and the start Pushbutton (PB2) is
momentarily depressed. When Control Power is off the machine is in an off state, however
some components in the electrical cabinet are still energized including the main fuses FU1 and
FU2, the Control Power Transformer (XFM1), fuse FU3, and wires 102 and 103 on the Stop
and Start Pushbuttons. Additionally, the Filter is powered by L11 and L21 and the Filter passes
power on wires L23 and L24 to contacts on the contactors C1 and C2.
Should main power be lost to the machine when the Control Power circuit is on, the Control
Power circuit turns off and stays off until power is restored and the start Button is pressed. This
prevents the machine from re-starting without operator action after any removal of power which
could occur with a brownout or momentary loss of power to a storm or power distribution
problem.
Transformer XFM1 reduces the incoming voltage from a nominal 230 (or 220) VAC to a
nominal 115 (or 110) VAC. 115V control circuits are industry standard in North America (this
allows the use of readily available Pushbuttons, Contactors, and other control circuit
components).
32397 Rev C1-2
9-29
Using Tormach PCNC 1100 Series 3
Warranty, Specifications, Customization and Troubleshooting
Figure 9.23 - Control Power Sub-system Portion of the Electrical Schematic
If your wall breaker consistently trips whenever you power up the Spindle (see section 9.6.5. 5)
than you should verify that the main machine power is not coming through a Ground Fault
Circuit Interrupt devise (GFI or known as RCCB in Europe) as the filters in the spindle drive
can allow minor leakage current to ground that, while considered safe, may also be sufficient to
trip a normal GFI beaker.
Figure 9.24 – Machine Cabinet Component Locations for Control Power
Using Tormach PCNC 1100 Series 3
9-30
32397 Rev C1-2
Warranty, Specifications, Customization and Troubleshooting
9.6.5.3
Computer Control Communication Sub-Section
Overview
Figure 9.25 – Computer control communications
The Mach3 Software is the machine control software for the PCNC. It allows for manual
jogging of the X,Y,Z, and A axes, the spindle speed, and the coolant pump through the
computer interface. It also allows the machine to run automatically with user supplied
programs. The Mach 3 Software runs on a Personal Computer and communicates with the
Tormach Machine Control Board to provide machine control. The “computer LED” on the
machine operator panel must be illuminated before the computer can control the machine.
32397 Rev C1-2
9-31
Using Tormach PCNC 1100 Series 3
Warranty, Specifications, Customization and Troubleshooting
Problem Resolution Checklists for the Computer Control Communication Sub-Section
Computer Control Communications Sub-system Checklist
Table 3.1
Computer Communication cannot be established
(computer LED cannot be turned on)
Possible Cause
Control Power is off
Ribbon Cable J4
between bulkhead
connector and the
Machine Control Board
not plugged in
Parallel Port cable is
not connected properly
between the computer
and the machine
Parallel port assignment
incorrect
Probability
Medium
Medium
Action to identify Cause
of Problem
Turn on Control Power
Check the connections on
both ends and ensure they
are firmly seated
Discussion
Medium
Check the cable
connections. Check the
cable for damage.
You may want to try a new cable if
you have one
Low
Consult the PCNC
Manual, section 9.5.9,
Using a Non-standard
printer port
If you supply your own computer
you will most likely need to
configure the port.
This problem is unlikely if you
purchased the computer from
Tormach
You may have to perform the step
above
This is by far the least likely problem
or
High
Parallel Port bad
Low
Tormach Machine
Control Board defective
Low
Try a new parallel port
card
Swap boards
See Control Power Sub-section
The connection at the Control Board
has been known to loosen up during
shipping.
Details of the Computer Control Communication
Mach3 software is installed under Windows XP or Windows Vista. The software allows the
user to jog or position the X,Y,Z, and A axes and to control the spindle speed and coolant pump
operation by use of the keyboard, mouse, and the jog/shuttle control. The software also accepts
G-code programs that automatically control the machine.
The Windows computer’s parallel port communicates with the Tormach Machine Control
Board through via a printer cable which has 25 pin D connectors on each end. In order for the
computer to control the machine, the Mach3 software application must be running, the machine
LED must be on, and communication must established between the computer and the Control
Board. Communication is established by clicking the “Reset” button in the Mach3 software
when the “Machine OK” indicator in on the Mach3 screen is solid green. This will cause the
bar indicator above the “Reset” button to change from flashing green to solid green and will
also turn on the “computer LED” on the machine operator panel. Once communication is
established the Mach3 software can control machine operation.
Note: The Spindle can be controlled via the computer or manually via the operator panel
controls—see figure 9.22. The “manual / auto” rocker switch must be in the auto position for
computer control of the spindle.
Using Tormach PCNC 1100 Series 3
9-32
32397 Rev C1-2
Warranty, Specifications, Customization and Troubleshooting
9.6.5.4
Axes Drive Sub-system
Figure 9.26 – Axis drive arrangement
Overview of the Axis Drive Sub-system
DC Stepper Motors are used to move the X,Y,Z (Z axis vertical travel, not rotation), and A
axis. The motors are powered by electronic driver modules (also referred to as axis drivers or
stepper drivers) which receive control signals from the Tormach Machine Control Board. The
electronic driver modules get power from the DC Bus Board. Motion is limited in the extremes
of travel by end of travel limit switches.
The next section is a Problem Resolution Checklist section which is presented in a table
format.
32397 Rev C1-2
9-33
Using Tormach PCNC 1100 Series 3
Warranty, Specifications, Customization and Troubleshooting
For more in depth explanation of this subsystem, please go to the Details section that is after
the Checklist section.
Problem Resolution Checklists for the Axis Drive Sub-system
Contents of the Problem Resolution Checklists for the Axis Drive Sub-system
Table 4.1
None of the Axes will move when Commanded
Table 4.2
One axis will not move or moves in only one direction,
but other axes operate properly
Table 4.3
Stepper Motor Winding Resistance
Table 4.4
DC Bus Power Distribution
Table 4.5
Axis movement is extremely noisy
Table 4.6
Cannot Reference all Axes or End of Travel Limits don’t Work, aka Limit Switch
Problems
Table 4.7
Testing Limit Switch Problems
Table 4.8
Steps are lost on Axis Travel
Possible Cause
Software not
commanding the move
or computer problem
Control signals not
reaching the electronic
driver modules
Axes Drive Sub-System Checklist
Table 4.1
None of the Axes will move when Commanded
ProbAction to identify Cause
Discussion
ability
of Problem
High
Jog the axis and observe
If the displayed position does not
the machine coordinate
change while jogging there is a
display
software/computer problem. Try
restarting the software first. If that
does not solve the problem, try
restarting the computer.
Medium
Problem with 25 pin Dconnector cable from
computer to machine
Problem with cable bottom
of machine cabinet to
Tormach Machine Control
Board
Problem with cable from
Tormach Machine Control
Using Tormach PCNC 1100 Series 3
9-34
32397 Rev C1-2
Warranty, Specifications, Customization and Troubleshooting
A malfunction of the
DC Bus
32397 Rev C1-2
Low
Board to Axis Drives
Troubleshoot using the
information in the Details
section
9-35
Using Tormach PCNC 1100 Series 3
Warranty, Specifications, Customization and Troubleshooting
Figure 9.27 – Diagnosis by swapping two axes
Axis drivers are mounted left to right in the sequence X, Y, Z A.
Using Tormach PCNC 1100 Series 3
9-36
32397 Rev C1-2
Warranty, Specifications, Customization and Troubleshooting
Axes Drive Sub-System Checklist
Table 4.2
One axis will not move or moves in only one direction,
but other axes operate properly
Possible Cause
Probability
High
Action to identify Cause
of Problem
Investigate connections
Discussion
Loose Wires or
Ribbon Cables
High
Turn on power after completion and
check for operation.
A loose coupling on
the motor
Medium
A bad Electronic
Driver Module
Medium
Remove power and check
the ribbon cable and the
wires from the DC Bus
Board
Jog the axis and listen to
determine if you can hear
the motor run
Swap the ribbon cable
connector for the control
signals, and the motor/AC
supply connector between a
known functioning drive (X
Axis in figure 9.27) and the
malfunctioning drive (Y
Axis in figure 9.27)
NOTE! Do not swap any
wires on a live system.
Power down first or
damage may result!
Parallel Port cable not
fully plugged in or pin
bent on connector
Jog the Y axis in both
directions
Jog the X axis in both
directions
32397 Rev C1-2
9-37
If not tightened down, parallel cables
will come loose, also look for any
bent pins at the connection point.
Remove the cover plate over the
coupling and observe if the motor is
turning but the screw is not.
Since there are at least 3 identical
electronic driver modules in the Axis
Drive Sub-system, swapping control
signals between modules is very
helpful during troubleshooting. One
must recognize that if control signals
are switched from the electronic
driver modules on the non-functioning
axis to a module on a functioning
axis, the end of travel limit switch on
the non-functioning axis will not
work. Take care to avoid reaching the
end of travel when moving an axis.
If the X axis moves properly, the
control signals are good then it is
likely the Y axis driver is bad
If the Y axis does not move or moves
in only one direction, a bad Y axis
driver is confirmed
If commanding the X Axis moves the
Y Axis, it's likely there was a poor
connection in the ribbon cable
connector to the axis driver module.
Swap the ribbon cables back and
repeat the test. Inspect the ribbon
cable connectors. “Wiggling” them
may be worthwhile to try.
It is also possible that there is a
damaged Ribbon Cable J4, parallel
port cable, or parallel port card in the
control computer.
Using Tormach PCNC 1100 Series 3
Warranty, Specifications, Customization and Troubleshooting
Axes Drive Sub-System Checklist
Table 4.2 (continued)
One axis will not move or moves in only one direction,
but other axes operate properly
A bad motor or motor
Low
Power down and remove
Simply unplug the power connector
connection
the motor leads from the
from the board
Axis Drive.
Measure the resistance of
Note: When making resistance
the windings of the motor
measurements on motors and other
per Table 4.3
devices with low resistance, always
take a tare* reading on the meter
before doing the resistance
measurement on the motor or device.
See “Measuring Resistance” in the
“Using the digital Multi meter for
electrical tests” section
If the resistance is out of
If unsure about the wiring it is best to
range, check the wiring
disconnect the motor leads from the
carefully. If the wiring is
wiring and measure resistance at the
good and the resistance
motor. You can also check the wiring
readings are out of range,
(which is now disconnected) for
the motor is bad
shorts wire to wire and wire to
ground and also for wire breaks.
A blown fuse on the
Low
Monitor DC Voltage from Note that a blown fuse usually is the
DC Bus Board
the DC Bus Board
result of a bad drive. If you replace a
fuse and it immediately blows,
Refer to Table 4.4
suspect a bad stepper drive or wiring
to the drive.
Mechanical Problem
Low
Gibs too tight or too loose
Oil not getting to the ways
and ball screw.
Thermal Trip on a
Drive
Low
Electrical Short on a
Drive
Low
Using Tormach PCNC 1100 Series 3
Oil residue from long term
storage
Debris on ball screw
Look at the LED's on the
stepper drivers. If there is
a red LED lit on the drive,
then it has tripped.
Look at the LED's on the
stepper drivers. If there is
a red LED lit on the drive,
then it has tripped.
9-38
Adjust using procedure in section
9.5.5. Note: Too tight results in too
much friction in the system. Too
loose can cause binding.
Investigate oiling system for lack of
oil and/or plugged lines. Refer to
Service Bulletin SB0031.
Repeatedly pump oil and slowly jog
axis or axes
Clean ball screw
Cycle power to the machine, and the
trip should reset. If it persists, then
try a new drive.
Cycle power to the machine, and the
trip should reset. If it persists, then
inspect the wiring for shorts, test teh
motor resistance by using table 4.3 or
try a new drive.
32397 Rev C1-2
Warranty, Specifications, Customization and Troubleshooting
X Axis
From To
Table 4.3 Stepper Motor Winding Resistance
Y Axis
Z Axis
A Axis
From To
From
To
From To
(Black
Probe)
(Red
Probe)
(Black
Probe)
(Red
Probe)
(Black
Probe)
(Red
Probe)
(Black
Probe)
(Red
Probe)
308
309
310
312
313
314
316
317
318
320
321
322
322
323
321
310
309
314
313
318
317
Resistance
Ω
Above
Tare*
0.5-2.0 Ω
0.5-2.0 Ω
>1 M Ω
0.5-2,0 Ω
>1 M Ω
Note, resistance across leads on all phases for X, Y and Z
should be about the same. Deviation may indicate a
problem. This does not apply to A axis.
All
Wires
Above
Ground
Bar
All
Wires
Above
Ground
Bar
All
Wires
Above
Ground
Bar
All
Wires
Above
Ground
Bar
>1 M Ω
Table 4.4 DC Bus Power Distribution
The DC Bus Board contains 4 fuses which are used to individually fuse power to the stepper driver
modules. A 5th fuse is provided on the Supply Boards for the Z axis Brake. Fuses are noted on the circuit
board. Note that the control power circuit must be on (“Machine” LED is on).
Fuse Number
on DC Bus
Board
F1 X
F2 Y
F3 Z
F4 A
F5 Brake
32397 Rev C1-2
Function
X axis
Y axis
Z axis
A axis
Brake for Z axis
Wire Numbers to
Monitor with Common
Lead (0V) listed first
303 302
305 304
307 306
325 324
327 326
9-39
Voltage when DC Bus is OK
and when fuse is good
55-75VDC
55-75VDC
55-75VDC
55-75VDC
55-75 VDC
Using Tormach PCNC 1100 Series 3
Warranty, Specifications, Customization and Troubleshooting
Possible Cause
Bad Capacitor for DC
Bus Board
Axes Drive Sub-System Checklist
Table 4.5
Axis movement is extremely noisy
ProbAction to identify Cause
Discussion
ability
of Problem
Low
Turn off control power,
and unplug the lower
connector (contains 5
wires all labeled with 300
series numbers) from all of
the electronic axis
modules.
With the cabinet door
Observe the green LED on the DC
open, turn on control
Bus Board illuminate.
power
While observing the green If the LED extinguishes in 2 seconds
LED on the DC Bus
or less, the capacitor is bad and must
Board, press the Stop
be replaced.
button.
If the LED takes 5 seconds or more
to extinguish, the capacitor is good.
If the results are not
conclusive, turn off
Control Power and unplug
the power connectors from
the axis drives
Turn on control power and
measure DC voltage on
wires 300 (common) and
301.
Turn off Control Power
and plug the power
connectors back on the
axis drives
Turn off power and tighten
all screw connections
Loose wire connection
High
Bad stepper driver
module
Medium
See Table 4.2
Wrong version of Mach
3 for given machine
configuration
Failing control
computer, or control
computer not suited for
M3
Loose Sheet Metal
Medium
Contact Tormach Support
Low
Run DriveTest.exe found
in the c:\pcnc3 folder
High
Feel for vibrating sheet
metal.
Using Tormach PCNC 1100 Series 3
9-40
A DC voltage of a nominal 65 VDC
(55-75) indicates the capacitor is OK
A DC voltage of a nominal 40 VDC
(35-45) indicates the capacitor is
defective.
There have been cases of a noisy axis
relating to a bad driver. This may be
temperature dependant.
Some versions of Mach 3 release by
Tormach are not compatible with all
machine configurations
A Flaky computer, or one that is not
suited to run real-time software such
as Mach3 will not produce smooth
step signals for good axis motion.
Often loose sheet metal is mistakenly
diagnosed as a noisy stepper motor.
32397 Rev C1-2
Warranty, Specifications, Customization and Troubleshooting
Squeaky Z axis brake (Z
axis only)
32397 Rev C1-2
Low
Noise will be noticed
coming from the brake
canister
9-41
On some systems, certain stepper
motor speeds can cause excessive
vibration in the sheet metal stands.
Identify the problem areas and treat
with silicone caulk.
Removing the brake (Caution, the
brake wires are short and somewhat
fragile –lift the brake canister off the
motor with caution!!!) and placing a
dab of grease on the motor spindle
shaft and on the shafts mating
surface on the under side of the brake
will remove excess noise without
compromising the brake’s function.
Using Tormach PCNC 1100 Series 3
Warranty, Specifications, Customization and Troubleshooting
Axes Drive Sub-System Checklist
Table 4.6
Cannot Reference all Axes or End of Travel Limits don’t Work
aka
Limit Switch Problems
Possible Cause
ProbAction to identify Cause
Discussion
ability
of Problem
Limit Switch Stuck in
High
Consult the Diagnostic
See Table 4.7
the on state
Screen in the Mach3
Software to see if a Limit
Switch is being reported as
Or
actuated even though no
axis is at the end of its
Limit Switch wire
travel
broken or wire
connection bad
Limit Switch contacts
Medium
Consult the Diagnostic
See Table 4.7
stuck in the off state
Screen in the Mach3
Software to see if a Limit
Switch is being reported as
not actuated even though
the axis is at the end of its
travel
Limit Switch not being Medium
Check to see if the limit
If it looks like the switch is being
contacted at end of
switch loose or if the
actuated properly but the diagnostic
travel
actuating cam is actually
screen does not report the switch as
contacting the switch
being made, go to next step,
Control Board
Low
See Table 4.7
A defective control board will report
Defective
no change in the state of the limit
switch even though the switch and
wiring are functioning properly.
Using Tormach PCNC 1100 Series 3
9-42
32397 Rev C1-2
Warranty, Specifications, Customization and Troubleshooting
Diagnostic Screen Inputs
Status Reported
“X Limit and Home” light is
always on even though the
switch is not actuated
“Y Limit and Home” light is
always on even though the
switch is not actuated
“Z Limit and Home” light is
always on even though neither
the up or down limit switch is
not actuated
“X Limit and Home” light is
never on even though the switch
is actuated
“Y Limit and Home” light is
never on even though the switch
is actuated
“Z Limit and Home” light is
never on even though either the
up or down limit switch is
actuated
Axes Drive Sub-System Checklist
Table 4.7
Testing Limit Switch Problems
Test to Perform
Results and Conclusions
on Wiring at the
Control Board
Jumper J2-1 to
If the light does not go out when the terminals
are jumpered, the Control Board is defective.
J2-4
Jumper J2-2 to
J2-4
Jumper J2-3 to
J2-4
Remove wire
J2-1
Remove wire
J2-2
Remove wire
J2-3
If the light goes out when the terminals are
jumpered, the wiring has a break or the limit
switch is defective. Remove power from the
machine, disconnect wires from the switch and
tie the two wires together and tape over to
prevent short circuits. Apply power. If the
diagnostic light is off, the wiring is OK and the
switch is bad. If the diagnostic light is on, the
wiring has a break or bad connection.
If the light does not go on when the wire is
removed, the Control Board is defective.
If the light goes on when wire is removed, the
wiring has a short or the limit switch is
defective. Remove power from the machine,
disconnect wires from the switch and tape the
end of each wire to prevent shorts. Apply
power. If the diagnostic light is on, the wiring
is OK and the switch is bad. If the diagnostic
light is off, the wiring has a short circuit.
Please note: often times a defective switch can be cleaned (blow out with compressed air) and
sprayed with WD-40 to fix a problem.
Please note: On some machines, the stainless steel bed pan does not sit tight against the front
edge of the mill bed; this allows coolant and chips to converge on the X-limit switch. Using a
bit of silicon sealer between the pan and bed will prevent this from occurring.
Details of the Axis Drive Sub-system
Motion for the X,Y,Z, and optionally the A axis are provided by DC Stepper Motors. Each
motor is powered by an electronic driver module. The driver module receives nominal 65 VDC
power from the DC Bus Board and receives control signals from the Tormach Machine Control
Board which processes and formats information sent by the control computer.
Find the relevant portion of the electrical schematic highlighted below. You may find it helpful
to have your electrical schematic available to use along with this discussion.
32397 Rev C1-2
9-43
Using Tormach PCNC 1100 Series 3
Warranty, Specifications, Customization and Troubleshooting
Axes Drive Sub-System Checklist
Table 4.8-Steps are lost on Axis Travel
NOTE! It is advised to also consult Table 4.2 as the information there will also apply to lost steps.
Possible Cause
ProbAction to identify
Discussion
ability
Cause of Problem
Improper use of tool
High
See Machine Position
By far the most common cause of a
offset (G43), Work offset
Test described after this perceived "loss of position" or "lost
(G54-59), or cutter
table.
steps" is user error. Please refer to
compensation (G41-42)
Chapter 7 for details on using machine
offsets in Mach.
Spindle tooling not
High
Inspect to insure the
properly locked down (Z
cutter is not slipping in
axis only)
the holder or that the
tool holder is not
pulling out of the collet.
Motor Coupling loose or
Low
Inspect
You may find it useful to run the axis
cracked
with the cover removed. A paint line
from shaft, through coupling to screw
can be used to see if there is any
movement over time. Use caution; keep
away from the rotating parts.
Holding Brake not
Low
Z will usually move
You should be able to hear motor
releasing (Z axis only)
down properly but will cogging whenever you tell the axis to
not move up
move. It should be noted that usually,
the brake alone does not have the torque
to cause a loss of step. Typically a
condition such as poor lubrication
combined with a bad Z brake are
required to actually lose position.
Computer or Software
problem
Obstruction or excessive
friction (gibs not adjusted
properly or poor
lubrication) or high load
in the mechanical system
Low
Restart the application
software first. If no
success, then restart
both the computer and
the application
software.
Low
Re-install Mach 3 after
downloading current
version from the
Tormach website, for
your machine
configuration.
Low
Jog the axis with the
jog/shuttle control and
carefully observe the
motion.
Using Tormach PCNC 1100 Series 3
9-44
It may be required to swap out the
computer, especially if you have
observed other glitches with the
computer. It is possible the computer
being used is not up to the task of
running real-time machining software
such as Mach.
If the wrong version of Mach 3 is being
used for your particular machine
configuration, loss of position is
possible.
It has happened, on rare occasion, that
Tormach mistakenly sent out versions
of Mach 3 with an improper
configuration file. downloading the
latest version from our website will
eliminate the possibility of this problem.
If you lose steps, it is normally many
steps. You should be able to hear the
motor cogging; Mechanical issues most
often result in losing a large number of
steps or stalling. Typical mechanical
issues include an increase in friction due
32397 Rev C1-2
Warranty, Specifications, Customization and Troubleshooting
to lack of oil at the way surfaces or ball
screw and/or improperly adjusted gibs.
They also come from excessive load on
the system due to chips or debris on the
way surfaces or ball screw, a sticking Z
axis brake or an end-of-travel bumper
wedged against the motor mount casting
(this occurs sometimes after a limit
switch failure and is more common on
the Z axis)
Stepper Drivers have
wrong DIP switch
settings
Low
See electrical schematic
in the back of the
manual. Note: new
steppers from Tormach
will require the user to
set these DIP switches
at installation.
Additional Notes on Lost Steps
In the spirit and philosophy of this guide, "divide and conquer" has no better application than in
the case of trouble shooting loss of position, or "lost steps". Please note, that as a general rule, a
properly operational Tormach PCNC being used in overloaded cutting situations, should
experience a spindle stall (or a broken cutting tool) long before an axis sees so high a cutting
force that it stalls or skips. Keeping this in mind, it is worth mentioning that the vast majority of
problems that are mistakenly associated with "lost steps" are actually due to one or more of the
following:
1. Improper use/call-out of machine offsets such as G54/55 as well as G43
2. Tool pull out as a result of a cutter or holder not secured properly
3. The wrong diameter tool used in the CAM program (i.e. many 1/2" end mills aren't actually
.500 inches).
4. Machine referencing to the part was performed improperly and/or relying on the end of
travel limit switches to set machine offsets.
5. Fixturing does not secure work, or does not facilitate repeatable mounting of work from one
piece to the next.
These are what we call Process Errors and have little to do with a problem residing with the
machine itself. The scope of this portion of the trouble shooting guide does not cover solutions
to process errors.
It is imperative to "Divide" a given set up into manageable portions so one can focus on where
the problem really lies... is it a process problem, or is it a machine problem? In order to isolate
machine problems from process problems, the "process” must be removed from the set up. The
point of this test is to measure the machine motion explicitly, thus eliminating process based
problems. This test is written for checking the X- axis, similar process can be used on Y and Z
as well.
1. Be sure that G40 and G49 show up in the modals list at the top of the screen
2. Mount a quality dial indicator on the mill bed, orienting the plunger along the X-axis. Place
near the end of travel.
3. Orienting the axis such that the indicator plunger contacts an appropriate surface on the
spindle head, move the X axis such that the indicator is zeroed, then zero the X-axis DRO.
32397 Rev C1-2
9-45
Using Tormach PCNC 1100 Series 3
Warranty, Specifications, Customization and Troubleshooting
4. After moving the spindle head away from the indicator , proceed with “exercising” the axis.
This means, using manual moves, or a very simple G-code program, move the axis at
varying speeds, particularly rapid speed. The more steps you run the axis through, the
higher the probability that a step will be missed, if there is indeed a machine problem.
5. Return the axis to indicator zero, and read what the DRO says. Allowing for some lost
motion (about .001”), the value indicated on the DRO should be 0. If not, then the machine
is indeed missing steps.
Figure 9.28 – Axis drive subsystem portion of schematic
When Control Power is on, contacts from contactor C1 pass the nominal 230 VAC input power
to XFM2, the DC Bus power transformer. XMF2 reduces the voltage to a nominal 48VAC
which is sent to the DC Bus Board on wires L15 and L25. A full wave bridge rectifier on the
DC Bus Board in conjunction with a 15,000 μF (micro-Farad) capacitor connected (wires 300
{common} and 301) to the DC Bus Board provide a nominal 65 VDC supply for the electronic
driver modules which can be measured on wires 300 and 301. This supply is individually fused
for each axis and distributed to each axis as noted in Table 4.4 above.
Using Tormach PCNC 1100 Series 3
9-46
32397 Rev C1-2
Warranty, Specifications, Customization and Troubleshooting
Figure 9.29 - Machine Cabinet Component Locations for the Axis Drive Subsystem
Control signals to move the axes are created by the Mach3 software in the control computer.
The computer sends the axis commands via the parallel port to the Tormach Machine Control
Board which massages these signals and distributes them to the individual axis commands
through a ribbon cable which plugs into the axes drives.
The X,Y and Z Axes each have 1 limit switch which actuates at the end of travel in each
direction. These limit switches are used to stop the travel of an axis before the mechanical limit
is reached. The limit switches are also used to stop an axis near its extreme travel position
during a reference procedure.
Sensors such as limit switches are usually the biggest source of problems on a machine. By
necessity they need to be mounted out on the machine where they are detecting events such as
end of travel. This makes them vulnerable to damage. They can get fouled by coolant, chips, or
by physically being contacted. Sticking is also a common problem as is wire damage.
The PCNC electronics are such that if any one limit switch is actuated, or the Control Board
thinks the switch is actuated, the other limit switches will not function to stop travel, even
though the respective end of travel limit switch is contacted. Additionally, if one switch is
actuated, the “Reference All” button will not cause all of the axes to be referenced.
The limit switches are all wired normally closed. Therefore, a broken wire or bad connections
results in the Control Board detecting a limit switch is actuated.
The diagnostic screen shows the status of the switches.
The axes are driven by stepper motors that have no feedback. It is possible that an axis can be
commanded to move but will not move as far as it is commanded to. This is commonly referred
to as “loosing steps”. Excessive friction or load in the mechanical system will cause loss of
steps. When loosing steps it is usually possible to hear a cogging noise from the motor. The
probability of losing a single step or just a few steps from a mechanical problem is very low.
Mechanical issues most often result in losing a large number steps or stalling the motor.
Tormach has found that loosing steps is usually due to the software or the computer. Appearing
to lose steps on the Z axis is frequently due to the tool holder being pulled out of the collet or
the cutter slipping in the holder.
32397 Rev C1-2
9-47
Using Tormach PCNC 1100 Series 3
Warranty, Specifications, Customization and Troubleshooting
9.6.5.5
Spindle Drive Sub-system
Overview
The Spindle on the PCNC is powered by an AC motor whose speed is controlled by a variable
frequency drive (VFD).
Figure 9.30 – Spindle Drive subsystem
Using Tormach PCNC 1100 Series 3
9-48
32397 Rev C1-2
Warranty, Specifications, Customization and Troubleshooting
Figure 9.31 – Operator spindle control components
With Control Power On, the Spindle Lockout Keyswitch On, and the Spindle Drive Door
closed, the drive is in a ready to run condition.
When the Manual Auto Switch is in the Manual position, the drive is turned on and off with the
Start and Stop Rocker Switches. The Speed Pot will then control motor speed.
When the Manual Auto Switch is in the Auto position, the machine control software provides
start, stop, and speed information based on user input.
You will find listed immediately below a Problem Resolution Checklist section. For more in
depth explanation of this subsystem, please go to the Details section that is after the Checklist
section.
32397 Rev C1-2
9-49
Using Tormach PCNC 1100 Series 3
Warranty, Specifications, Customization and Troubleshooting
Problem Resolution Checklist for the Spindle Drive Sub-system
Contents of the Spindle Drive Sub-System Problem Resolution Checklist
Table 5.1
Spindle will not turn in Manual or Auto
Table 5.2
Run and Direction Commands to Drive
Table 5.3
Spindle Will Not Run At High Speed
Possible Cause
No Power to Spindle
No Power to Drive
No Power to Drive
because Contactor C2 is
not energizing. This
can be checked by
checking the voltage
across L16 and L26 at
the drive.
Meter should read 200250 VAC
Spindle Drive Sub-System Checklist
Table 5.1
Spindle will not turn in Manual or Auto
ProbAction to identify Cause
Discussion
ability
of Problem
If the display on the drive is on,
proceed to “Belt is Loose or Broken”
The drive has power if the Note: When power is removed, the
digital display lights up.
drive display will remain active until
the internal capacitors dissipate their
energy, usually about 15 seconds or
so.
High
Spindle Lockout key
115 VAC measured from wire 100 to
switch off or defective
wire 105 when OK
High
Spindle Cover Door not
115 VAC measured from wire 100 to
holding Belt Guard switch wire 106 when OK
closed or switch defective
Medium
Loose wires in circuit
Turn off power and search for loose
wires. Re-apply power when
finished and check operation.
Low
Tormach Machine Control
Board not providing run
command or holding
contact on C2 between
wires 106 and 107 bad
Insure you have 115 VAC measured
from wire 100 to wire 106 (see
above). Make a jumper wire and
using proper care associated with
live circuits, momentarily jumper
wires 106 and 107. If Contactor C2
pulls in (you will hear an audible
clunk) while you have the jumper on
but drops out as soon as you remove
the jumper, the holding contact on
C2 is defective. If C2 stays
energized, the control board is not
passing the run signal to the circuit.
Make certain you are commanding
the drive to run. If so, the Tormach
Machine Control Board is defective.
In manual mode press the
stop rocker switch. With
the door open press the
start rocker switch and
listen for a soft audible
click on the control board.
If you hear this click (from
a relay contact on the
board), the board is
functioning properly.
Using Tormach PCNC 1100 Series 3
9-50
32397 Rev C1-2
Warranty, Specifications, Customization and Troubleshooting
Spindle Drive Sub-System Checklist
Table 5.1 continued
Spindle will not turn in Manual or Auto
Possible Cause
Drive has tripped
Probability
Low
Action to identify Cause of
Problem
The display will show if the
drive has tripped. Record
the information from the
display should the trip be
happening frequently or
should the trip not clear as
described in the Discussion
column to the right. The
display will look similar to
that shown to the right
Discussion
Drive trips may be cleared by
removing power from the drive for
30 seconds by use of the Spindle
Lockout Key Switch
The letters tr on the left side of the
display indicate a drive trip and the
letters on the right define the type
of trip.
See Table 5.3 “Spindle Drive
Trips” in the Details section for a
list of drive trips
Err 0 occurs
32397 Rev C1-2
Low
Check wiring to braking
resistor
9-51
Symptoms are spindle takes a long
time to slow down
Using Tormach PCNC 1100 Series 3
Warranty, Specifications, Customization and Troubleshooting
Possible Cause
Belt is Loose or
Broken
or
sheaves are not fixed
to motor or spindle
Defective Drive
Spindle Drive Sub-System Checklist
Table 5.1 continued
Spindle will not turn in Manual or Auto
Prob- Action to identify Cause of Problem
Discussion
ability
Low
Check the mechanical system
Turn off Disconnect Switch
before investigating
Low
Un/Mis-programmed
Drive
Low
Defective Tormach
Machine Control
Board
Low
or
Defective cables
between the Control
Board and the Spindle
drive
Using Tormach PCNC 1100 Series 3
If the display is not on and there is
nominal 230 VAC between wires L16
and L26, the drive is defective.
If the drive displays a trip
condition that does not clear
with removal of power, it is
possible the drive is bad.
Push the “M” button on the front
A drive reprogram is a simple
panel of the drive momentarily. The
operation, but requires a
display will change to 01___0.0 with
programming key from
the 01 blinking. Momentarily push the Tormach.
up arrow key to the right of the M
key, the 01 changes to 02. Take note
of the number to the right of the 02.
Your VFD should read ‘170.X’,
where ‘X’ designates the VFD
program version. If it does not display
this value than your drive requires
re‐programming. To exit this mode,
push and hold the M button until the
display reverts.
Check that all cables are seated
properly in their connectors on the
board
Attempt to run the drive. If the
If the display reads rd 0.0,
display reads Fr xy.z or Ld xy.z
measure DC voltage per Table
where xy and z are numbers between
5.2 below. Be sure to measure
0 and 9, the Control Board is sending at the Control Board and at the
a run (enable) signal to the VFD. A
drive to determine if there is a
reading of rd 0.0 indicates the drive
problem with the wiring. It is
is ready but not receiving a run
not critical that the
command.
measurement for reverse be
made as it is not required to
make the Spindle turn;
Note that the drive may be displaying however it may aid in further
numbers on the left side of the
trouble-shooting.
display. If the digits on the right side
of the display are flashing,
If your measurements match
momentarily press and release the M
button just below the display to cause those in Table 5.2, the Control
Board and wiring to the drive
the left side digits to flash. With the
are good.
left side digits flashing, press and
hold the M button for 3 seconds and
the display will change to Fr, Ld or
rd as described above.
9-52
32397 Rev C1-2
Warranty, Specifications, Customization and Troubleshooting
Defective Tormach
Machine Control
Board or cables
between the Control
Board and drive
Attempt to run in manual with the
Speed Pot in a mid-range position
Determination of Defective Drive or
Control Board
Defective Motor
Low
Power down the drive using the Key
Switch. Wait 30 seconds and measure
resistance between the leads of the
motor which are wire numbers 400,
401, and 402. Remember to take a tare
reading with your meter, See the
section on using your multi-meter in
the “Tips and Tools” section following
the “Philosophy of Troubleshooting.”
2-3.5 VDC measured on the
Control Board between wires
J1-2 (common) and J1-1
indicates the Control Board
speed output signal is OK.
Turning the pot from
minimum to maximum should
cause the voltage to range
from <1 to >4.5 VDC. Return
Pot to mid-position.
If the voltage measurements in
the two tests above are not
good, the Control Board is
defective; if correct the drive
is bad
Resistance should be in the
range of 2-4 Ω. 0 Ω would
indicate the winding is shorted
and >1M Ω would indicate the
winding is open, both cases
indicate a defective motor or
compromised wiring to the
motor from the drive.
Table 5.2a Run and Direction Commands to Drive
Command
From Card
Run
Reverse
Monitoring Points
One Probe on each
Common
Wire
Wire
Number
Number
J1-2
J1-2
J1-3
J1-6
Voltage Measured
Voltage when
Control Board
Command
IS on
20-28 VDC
0 VDC
Voltage when
Control Board
Command
IS NOT on
0 VDC
20-28 VDC
Table 5.2b Main Control Board LED Indicators for Run and Speed Commands to Drive
Mode
Setting
Indicator
Manual (front panel switch
Start button on front panel
Yellow LED D15 lights.
turned to "Manual")
engaged
Brightness proportional to
speed
Auto (front panel switch
turned to "Auto")
32397 Rev C1-2
Start button on computer
screen engaged
9-53
Yellow LED D15 lights.
Brightness proportional to
speed
Green LED D10 lights and
blinks at a rate proportional to
speed
Using Tormach PCNC 1100 Series 3
Warranty, Specifications, Customization and Troubleshooting
Details of the Spindle Drive Sub-system
Figure 9.32 – Spindle Drive Sub-system Portion of the Electrical Schematic
The relevant portion of the electrical schematic is highlighted in figure 9.32. You may find it
helpful to have your electrical schematic available to use along with this discussion.
Power is supplied to the drive through a contactor that allows power to pass when the drive is
commanded to run by the user. When the Mushroom Head stop button is pressed, or the when
Spindle Lockout Key Switch S7 is turned off, or when the Spindle Drive Door is opened,
Contactor C2 interrupts power to the VFD and prevents the motor from running.
Note: After a power down, the VFD will only power back up when first commanded to spin in
either manual or auto. The VFD will not power up simply upon pushing the green start button
on the Operator Panel. Once the VFD is powered up, it will stay powered until one of the above
conditions occurs.
Control signals are sent to the drive from the Tormach Machine Control Board which gets
commands from the computer in Automatic mode or from the Operator Panel in Manual mode.
When Manual is selected with the Manual Auto Rocker Switch, the start and stop Rocker
Switches, the forward / reverse Rocker Switch and the Speed Pot are used to control the Spindle
speed. In the Auto mode, none of these controls are functional and all control for the spindle is
provided by the Computer and machine control software.
The Tormach Machine Control Board provides a contact closure between wires 106 and 107 to
cause power to be applied to the drive. It also provides a run command, a direction command,
and an analog voltage in the range of 0-5 VDC to wires J1-1 (com) and J1-2 proportional to
desired speed. See the Problem Resolution Checklist for the Spindle Drive Sub-system,
Table 5.1, and Run and Direction Commands, Table 5.2, above.
The display on machines provides valuable information for troubleshooting. The display will
provide diagnostics which include:
Using Tormach PCNC 1100 Series 3
9-54
32397 Rev C1-2
Warranty, Specifications, Customization and Troubleshooting
•
Frequency output (proportional to speed. Range is ~7 HZ to 142 HZ)
•
Load in percent (Load is proportional to the torque the motor is outputting)
•
Status (rd for ready, ih for inhibit which will occur when there is no jumper between terminals
B2 and B4 on the drive)
•
Fault information (letters tr {for trip}) and a code for the fault
There are several trips that are worthy of note shown in the table below
Table 5.3
Trip Code
Condition
UU
OU
DC Bus Under voltage
DC Bus Overvoltage
OI.AC
VFD output instantaneous over
current
Braking resistor instantaneous
over current
I2t (power) on braking resistor
OI.br
It.br
It.AC
I2t (power) on VFD output
current (used to protect motor)
O.ht1
VFD has calculated it is working
too hard and needs to stop to
cool power electronics down to
prevent failure
Heat sink temperature is too
high because the VFD is
working too hard and needs to
stop to cool power electronics
down to prevent failure. Cabinet
may also be too hot.
Cooling fan not cooling
O.ht2
Hf.29
32397 Rev C1-2
Spindle VFD Trips
Likely Cause
This happens every time the VFD is powered down
Braking Resistor failed open or wiring connection
open between the VFD and the resistor
Phase to phase or phase to ground short on output of
VFD to motor
Braking resistor shorted or partially shorted out or
short in wiring between the VFD and the resistor
Excessive braking resistor energy caused by too
frequent and too severe deceleration cycles
or
AC supply voltage too high
You are working the spindle motor too hard.
Consider running the spindle motor at half speed for
10 minutes with no load to cool the motor down.
You are working the spindle motor too hard. Stop
running the spindle but leave the VFD power on and
let the power electronics cool down.
You are working the spindle motor too hard or it is
too hot in your shop. Stop running the spindle but
leave the VFD power on and let the power electronics
cool down. Check to see if the fan on the VFD is
running and check your filters on the cabinet. Cool
your shop down if required.
Failed drive.
9-55
Using Tormach PCNC 1100 Series 3
Warranty, Specifications, Customization and Troubleshooting
The drive can also provide parameter information. This is information from the Tormach
program of the drive and is usually not important from a user standpoint. If the drive is
displaying this sort of information, which always has 2 digit numbers displayed on the left side
of the display, the user must take action to allow the drive to display the diagnostic information
(above).
If the right side digits are flashing, momentarily press and release the M button just below the
display to cause the left side digits to flash. Now with the left side digits flashing, press and
hold the M button for 3 seconds and the display will change to display diagnostics.
If frequency is displayed and it is desired to display load, or vice versa, press and hold the M
button for 3 seconds.
Tormach highly recommends against changing any parameter values in the VFD, There are no
user settable parameters available.
9.7
Mechanical maintenance
The mechanical design and assembly is conventional in all aspects. Adjustments should be
simple to make, but rarely needed. The exploded views are your primary resource for
understanding assembly and adjustment. We encourage you to contact Tormach if additional
information is needed. Specific items to be aware of include the following:
•
The Z-axis is held up by the Z-axis ballscrew and motor. Decoupling the motor will
result in a dangerous and destructive fall, with the entire spindle head crashing into the
table.
•
X-, Y- and Z-axis ballscrews are mounted on angular contact bearings. The preload
adjustment on these bearings affects the axis backlash and bearing wear. Spanner
wrenches are very helpful to adjusting the locknuts and setting the tension. Tormach
offers the correct spanner wrenches (PN 30485) if you need to adjust or replace these
bearings
•
X-, Y- and Z-axis ballscrew nuts are preloaded using precision ground spacers. These
are factory set and cannot be adjusted.
•
X-, Y- and Z-axis slide ways each have a tapered gib plate, locked in place at each end.
Tapered gibs can act as wedges and jam the machine if the lock screws are not tight.
•
When correctly adjusted for preload, sustained high spindle speed will bring the spindle
bearings to about 155oF (68oC). This is a normal condition. Higher preload in the
spindle bearings will result in even higher temperatures and excessive wear.
•
Service Bulletin SB0024 covers the rebuilding of PCNC1100 spindle cartridges.
•
Major castings are fitted or scraped for precision fits and machine accuracy.
Exchanging parts between machines or replacing parts can affect the machine accuracy.
Dowel pins are used for alignment between parts. The dowel holes are drilled after
alignment between parts and are unique the original parts. Replacement parts cannot
use the original dowel holes.
The following tightening torques are appropriate to the metric fasteners used in the PCNC:
Using Tormach PCNC 1100 Series 3
9-56
32397 Rev C1-2
Warranty, Specifications, Customization and Troubleshooting
Diameter (mm)
9.8
Torque (Nm)
5
7
6
12
8
30
10
55
12
100
14
160
16
245
20
480
Electrical maintenance
Electrical Service: Certain service and troubleshooting operations require access to the
electrical cabinet while the electrical power is on. Only qualified electrical technicians should
perform such operations.
Many electrical problems are self-apparent. Tracing electrical problems can be done with a
combination of the machine control software, the LED indicators within the machine cabinet
and the machine actions.
The operating software has colored rectangular indicators, referred as LEDs, on various screens
to indicate output or functional status. The Diagnostics screen also has indicators for X, Y and
Z home/limit switches and accessory input status. These are useful to determine if the input is
operational.
There are also various physical LED indicators within the electrical cabinet. Among these are:
•
DC Power LED – Indicates voltage on the DC bus, power to axis drivers;
•
X-, Y-, Z- drivers – Green Indicate power to each individual drive. Red indicates a
Fault;
•
A-driver – Green indicates power to the drive;
•
Control Board LED1 – Indicates power to the control board;
•
Control Board D10 – Blinking indicates speed signal from software. Manual speed
demand is not shown.
•
Control Board D15 – Brightness indicates speed signal to spindle driver.
Beyond the obvious problems of broken limit switches, blown fuses and damaged motor cables,
we suggest contacting Tormach directly for advice on diagnosing or correcting electrical
problems.
9.9
Preparation for Transport
It will generally be straightforward to transfer the machine to a pallet and transport it in one
piece.
The Z-axis should be lowered and the spindle supported from the table on a box or solid block
of timber. The Z-axis should be under a relatively neutral force, not under stress by being
parked with a high downward force, nor held up by the ballscrew. Run it down to a wooden
block, but do not crunch it hard into the block.
If required, the stepper motors for the axes can be removed following the reverse of the
procedure described for installing the Y-axis drive. You can also remove the Z-axis motor to
32397 Rev C1-2
9-57
Using Tormach PCNC 1100 Series 3
Warranty, Specifications, Customization and Troubleshooting
reduce the overall height of the machine. Take care to secure the motors after they are removed
so strain is not placed on the wiring.
All bare metal surfaces should be oiled before moving the machine as a means of protection
against condensation and corrosion.
9.10
Disassembly for Transport
Warranty is void if the machine is disassembled. Tormach recognizes that there are situations
where users need to disassemble their mill and has made provisions in the design of the mill to
facilitate this. Never the less, Tormach cannot be held responsible for alignment, precision and
operating functions after the machine has been disassembled. Test your machine before
disassembling it.
The major sub-assemblies of spindle head, column and base are bolted and dowelled together
so the machine can be separated into smaller components to meet very challenging transport
problems. Note, however, that this entails disconnecting wiring and the lubrication lines. We
recommend taking a very large number of photographs from all angles including detail
photographs of any wires or oil lines that will be take apart. Dowel pins must be removed
before the bolts on disassembly. Dowel pins must be installed before the bolts on assembly.
Tormach strongly recommends that all precision sliding and rotating joints remain intact during
disassembly. This means that you should not remove ballscrews, bearings or separate sliding
joints. For example, in reference to the head and column exploded view (drawing D40134), you
should not separate item 82 (Z-axis slide) from item 75 (column). Instead you should separate
item 19 (Head Casting) from item 82 (Z-axis slide).
Detailed advice should be sought from Tormach support.
Using Tormach PCNC 1100 Series 3
9-58
32397 Rev C1-2
Appendices
10.
Appendices
10.1
Appendix 1 – Not Used
10.2
Appendix 2 – Exploded Parts Views
The following pages identify the mechanical and electrical components of the PCNC, cross
referenced to part numbers.
32397 Rev C1-2
10-1
Using Tormach PCNC 1100 Series 3
PCNC 1100 Series 3 (32085)
Column and Head Assembly
Parts List for PCNC 1100 series 3 – Drawing D40202 (Upper Exploded) – Sept. 2011
ID
1
2
3
3A
4
5
6
6A
7
8
9
10
11
12
13
14
15
16
17
18
19
20
21
22
23
24
25
26
27
28
29
30
31
32
33
34
35
36
37
38
39
40
41
42
43
44
45
46
47
48
Number
30303
30304
30305
30306
30307
31198
31199
31217
31200
31201
31202
31203
30315
30316
30317
30318
30319
30320
30321
30322
30323
30324
30325
30326
30327
30328
30329
30330
30331
30332
30333
30334
30335
30336
30337
30338
30339
30340
30341
30342
30343
30344
30345
30346
30347
30348
30349
30350
30351
30352
Description
1
Lower spindle bearing
Screw M8x30
Spindle cartridge
2
Spindle cartridge assembly
Screw M5x12
Screw M3x12
Latch
3
Latch Kit
Nut, M3
Nut, M5
Screw M5x16
Screw M6x16
Motor cover
4
Upper spindle bearing
Nut M33x1.5
Screw M5x8
Screw 12x50
Pin 8x35
Washer 12mm
Washer 12mm
Head casting
Spindle motor base
Washer 10mm
Washer 10mm
Screw M10x30
Nut M6
Pin 5X35
Spindle lock
Spindle lock pivot
Spindle pulley
Nut M27x1.5
Screw M4x8
Motor pulley
Handle pin
Set screw M5X8
Spring 1x4.8x20
Adjustable base handle
Adjustable base pivot pin 6X45
Adjustable base spindle motor
Adjustable base clamp bolt
Pin
Spring 1x4.8x20
Adjustable base clamp handle
Spindle motor
Spacer
Key 8X40
Screw M12x45
Sleeve
Pulley washer
Screw M8x20
ID
49
50
51
52
53
54
55
56
57
58
59
60
61
62
63
64
65
66
67
68
69
70
71
72
73
74
75
76
77
78
79
80
81
82
83
84
85
86
87
88
89
90
91
92
93
94
95
Number
30353
30354
30355
30356
30357
32002
30359
30360
30361
30362
30363
30364
30365
30366
30367
30368
30369
30370
30371
30372
30373
30374
30375
30376
30377
30378
30379
30380
30381
30382
30383
30384
30385
30386
30387
30388
30389
30390
30391
30392
30393
30394
30395
30396
31204
31205
31206
30507
30506
30560
Description
Screw M6x30
Spring
Screw M6x40
Screw M6x60
Screw M5x20
Z axis step motor w/Brake
Screw M5x26
Washer 5
Washer
Clamping shaft collar
Nut M14X1.5
Lock washer 14mm
Cover plate
Screw M10x40
Z axis motor base
Pin 6x30
Screw M16x12
Screw M16
Spacer
Z ball screw cover plate
5
Z axis ball screw bearing
Spacer
Z axis ball screw upper bumper
Column cover plate
Spacer
Z axis way cover
Column
Screw M12x60
Pin 10X55
Z axis ball screw & nut
Washer 6
Z axis gib
Screw
Z axis slide
Z nut carrier
Z axis screw lower bumper
Belt 3V280 Gates
Unused
Spindle R8
Pin
Key 8X26
Lower spindle spacer
Cylindrical pin 4X16
Big washer 6
Z axis lower way cover Bracket
Pin, M6x35
Screw, M5x12
Drawbar for R8 taper
Drawbar for BT30 taper
Alignment washer for drawbar
1
Annular Bearing Engineering Council identification: DT7008/DT (double tandem pair- ORDERED AS A PAIR)
2
Spindle Cartridge Assembly for R8 includes callout numbers 1,3, 12,13,14,73, 87, 88, and 90. For BT30 Spindle Cartridge Assembly, use PN 30505
3
Latch Kit Assembly includes callout numbers 5,6,7
4
Annular Bearing Engineering Council identification: D7007C/DT (double tandem pair –ORDERED AS A PAIR)
5
Annular Bearing Engineering Council identification: ABEC7202B/P5
54
24
23
25
26 6
29
27
49 28
34 30 31 32 33
35 36 37
15
38
4
39
41
42
43
44
39
15
1
7
45
46
47
14
16
5
15
24
6
12
22
48
21
21
15
16
16
20
22
7
19
54
18
24
59
23
21
25
7
15
52
7
26
6
17
29
6
16
27
28
13
35
12
34
40
33
31
11
30
32
10
9
8
12
24
5
4
3
2
1
42
44 43
55
54 58
PCNC 1100 Series 3 (32085)
Base Assembly
(Tool Tray not shown)
57
56
60
40
53
27
11
51
38
15
50
Parts List for PCNC 1100 series 3– Drawing D40203 (Lower Exploded) – Sept. 2011
ID
1
2
3
4
5
6
7
8
9
10
11
12
13
14
15
16
17
18
19
20
21
22
23
24
25
26
27
28
29
30
1
Number
30397
30398
30399
30400
30401
30402
30403
30404
30405
30406
30578
30408
30409
31207
30411
30412
30413
30414
30415
30416
30417
30418
30419
30420
32001
30421
30422
30423
30424
30425
Description
Screw M6x25
Manifold
Base
X & Y axis rubber bumper
Washer
Nut M14x1.5
Screw M4x12
Pad block
Screw M6x40
Y axis cover mounting plate
Y axis front or rear way cover
Screw M6x16
Oil pump LK-8TL
X axis rubber bumper left
Screw M5x20
Screw
Y axis gib
Table slide
Mounting plate for X limit switch
Screw M5x8
Screw M5x10
Plate
Washer 5
Washer 5
X,and Y axis motor
X & Y axis motor coupling
Screw M5x16
X & Y ball screw cover plate
Washer 14
Washer 8mm
ID
31
32
33
34
35
36
37
37A
38
39
40
41
42
43
44
45
46
47
48
49
50
51
52
53
54
55
56
57
58
59
60
Number
30426
30427
30428
30429
30430
30431
32401
32402
30433
31208
31209
30436
30437
30438
30439
30440
30441
30442
30443
30444
30445
30446
31210
30448
30449
30450
30451
30452
30453
31211
31212
Annular Bearing Engineering Council identification: ABEC7202AC/P5
Description
Lock washer 8mm
Screw M8x40
Pin 8x30
X & Y axis spacer
X, Y axis bearing1
X axis ball screw & nut
X axis motor base
Table Tray (not shown)
Shaft clamp
Block, x axis
Screw, M4x8
Table
Screw 6x26
Washer 6
Pin 6X25
Filter screen
X nut carrier
Manifold
X axis gib
Sleeve
Y axis motor base
Bumper
Cover Plate
Y axis ball screw & nut
Screw M5x25
Block
Screw M5x8
Cover limit switch
Y axis carrier
Elec. Box
Cover Plate
PCNC1100 SERIES 3 ELECTRICAL SCHEMATIC
LABEL: COOLANT POWER
LABEL: COMPUTER
LABEL: COMPUTER MONITOR
connector on cabinet. External
connection is made to computer
DB25 MALE
I/O MOUNT PLATE
SW6
COOLANT SW5
COMPUTER
206
202
203
204
202
202
FU6 - 6 AMP
ALL THICK LINES = 14GA WIRE (BROWN/BLUE)
207
206
1
L01
(Brown Wire)
3
230 VAC LINE
NOTE: FU3 AND FU7
MOUNTED TO TRANSFORMER
2
L1
4
F2 - 7 AMP
L2
5
DISCONNECT
DISABLE
C1
BELT GUARD
106
L21
6
100
C1
30465
FU7 - 3.15-2.15 AMP
FU2 - 15 AMP
F1- 1 AMP
KEY SWITCH
104
103
102
FU1 - 15 AMP
L02
(Blue Wire)
30684
205
202
FU3 - 0.75 AMP
XFM1
L11
201
200
PB2
START
PB1
ESTOP
230/120 PRIMARY/SECONDARY
CONTROL POWER TRANSFORMER
SW7
FAN
Tormach Machine Control Board
30685
105
LS5
107
C2
MACHINE FRAME
BONDED TO EARTH GROUND
FILTER
PN 32350
C2
30465
100
100
230/48 PRIMARY/SECONDARY
L13
L23
C1
DC BUS POWER
L24
DC BUS BOARD
L25
30686
X+
X-
LED2
COMPUTER
48VAC
Y+
Y-
L15
CAP - 15,000 uF 301
XMF2
C1
F1, F2, F3, F4, F7, F8 - 8 AMP
F6 - 15 AMP
Z+
F5 - 2 AMP
LS2
LS1
Z-
+CAP
LS3
SW1 FWD/REV
A+
A-
-CAP
DB+
C2
300
C2
L16
Brake+
X LIMIT
BrakeDB- ATC+ ATC-
L26
(FUTURE ADDITION)
POWER DRAWBAR
(FUTURE ADDITION)
AUTOMATIC
TOOL CHANGER
Y LIMIT
Z UPPER
SW2 STOP
Brake RLY+ Brake RLY+
328
329
SW3 START
C1
ALL THICK LINES = 14GA WIRE (BLACK)
Connection Board
PN 32089
version 1.3
L14
LED1
MACHINE
326 (connects to J1-7 on control board)
(FUTURE ADDITION)
400
401
M1
A DRIVE
P1
402
P1
P1
403
P1
P1
404
P1
P2-2
P2-1
P2-3
P2-4
P2-5
P2-6
324
320
321
322
323
J6-19 thru J6-24
All control wires 18GA Wire (Blue)
T2 to J1-1
T1 to J1-2
B5 to J1-3
T5 to B2 to B4 to J1-4
B6 to J1-6
(J1-4 jumpered to J1-5)
T1 to LM1 (J1-2)
B1 to LM2
SW4 AUTO/MAN
327 330 (connects to J1-8 on control board)
Z DRIVE
325
P1
P1
P1
Motor
30199
P1
P1
P2-2
P2-1
P2-3
P2-4
P2-5
P1
J6-13 thru J6-18
Y DRIVE
307
P1
306
P1
316
317
318
Motor Wires
Brake Wires
Motor
32002
P1
P1
P1
305
304
P2-2
P2-1
P2-3
P2-4
P2-5
P1
J6-6 thru J6-12
X DRIVE
P1
P1
312
313
314
P1
Motor
32001
P1
P1
303
302
ACCESSORY
P2-2
P2-1
P2-3
P2-4
P2-5
308
309
310
Motor
32001
P1
J6-1 thru J6-6
POT1 (31041)
MANUAL SPEED
22
15
32
31
41
1
28
26
DC BUS
BOARD
32005
STEPPER
DRIVER
32000
STEPPER
DRIVER
32000
X AXIS
Y AXIS
STEPPER
DRIVER
32000
Z AXIS
STEPPER
DRIVER
30737 or
31234
A AXIS
(OPTION)
26
25
18,19
39
25
25
27
16
POT1
Fuse FU7
XFM2
(30459)
6
10
XFM1
31097
Fuse FU3
5
30
BRAKING RESISTOR
31049
4
TORMACH MACHINE
CONTROL BOARD
31045
Fuse F1
7
Fuse F2
VFD
31036
SEE MOUNTING
BOLT PATTERN
IN DETAIL
BELOW
12
13
21
42
33
40
37
38
35
36
I/O MOUNT PLATE
30210
11
2,3
34
7A
7B
17
14
20
9
Parts List for PCNC 1100 Series 3 – Drawing D40182 (Electrical Overview) – Sept. 2011
ID
Number
Description
ID
Number
Description
Number
Description
1
31120
Fuse FU71
20 31040 LED
30686
J6 cable (axis drivers)
1A 31213
Fuse Holder for FU7
21 31036 VFD Motor Driver9
30627
Flex Conduit 16 mm OD
2
30455
Fuse FU1, FU22
22 32005 DC Bus Board
30628
Connector for 16 mm flex
2A 30510
Double Fuse Block
22A 31655 DC Bus Fuse F1,2,3,4,7,810.1
30722
Flex Conduit 12 mm OD
3
3
30456
Fuse FU6
22B 31123 DC Bus Fuse F510.2
30723
Connector for 12 mm flex
3A 30511
Single Fuse Block
22C 32404 DC Bus Fuse F610.3
30728
Flex Conduit 10 mm OD
4
31119
Fuse FU34
24 31045 Machine Control Board
30729
Connector for 10 mm flex
4A 31213
Fuse Holder for FU3
25 32007 On-Off Rocker
30470
Tormach Logo -vinyl
5
31097
Transformer XFM15
26 32008 (On)-Off Momentary Rocker
32405
PCNC 1100 Logo -vinyl
6
30459
Transformer XFM26
27 32006 On–Off-On Rocker
30222
Label, Belt Position
7
31045
Machine Control Board
30 32097 Operator Console Assembly
30223
Label, Machine Safety
7A 31877
Control Board Fuse F17
31 32000 Stepper Driver
30224
Label, Dual Power Safety
7B 30182
Control Board Fuse F28
32 30626 Fan, 115 VAC
30225
Label, Retain Voltage Safety
9
30462
Estop PB1
33 31104 Terminal Block
30742
X & Z Limit Switch (non-sealed)
10 30463
Push button PB2
34 31049 Braking Resistor
31860
X limit Switch (sealed) 12
11 30464
Key switch with keys SW7
35 30177 AC Power Outlet
30461
Y Limit Switch
12 30466
Relay contactor C1
36 30166 DB25 Male - IDC11
30536
Y Limit Switch w/ enclosure
13 30466
Relay Contactor C2
37 30258 AC Power Inlet
30577
Spindle Door Switch
14 30467
Cabinet latch & key
38 30165 I/O Mount Plate
15 30468
Capacitor
39 30685 J3 cable (console)
16 32350
Filter
40 30684 J4 cable (computer)
17 31039
Accessory / Probe Port
41 30454 Disconnect switch
18 31041
Potentiometer
19 30181
Knob
1 Metric size is 5x20 mm, 3 amp. Use Bussmann GMD-3A, Littlefuse 239003.P, or Ferraz GSC -3A
2 Metric size is 10x38 mm, 15A. Use Bussmann KTK-15, Littlefuse KLK-15, or Ferraz ATM-15
3 Metric size is 10x38 mm, 6A. Use Bussmann KTK-6, Littlefuse KLK-6, or Ferraz ATM-6
4 Metric size is 5x20mm .75A. Use Bussmann GMD-750mA, Littlefuse 239.75P
5 Control Transformer is 230/115 - 100VA
6 Axis Power Transformer is 230/48 - 500VA
7 Inch size is 1.25x.25, 1 amp. Use JVP AGC 1
8 Inch size is 1.25x.25, 6.3 amp. Use JVP AGC 6.3
9 Preprogrammed with current PCNC software
10.1 Fuse for dc bus board, F1, 2, 3, 4, 7,8. Use Bussmann GMD-8A, Littlefuse 239008.P, or Ferraz GSC -8A
10.2 Fuse for dc bus board, F5. Use Bussmann GMD-2A, Littlefuse 239002.P, or Ferraz GSC -2A
10.3 Fuse for dc bus board, F6. Use Bussmann GMD-15A, Littlefuse 239015.P, or Ferraz GSC -15A
11 This component is included as part of the J4 cable, callout #40 PN30684
12 This is a sealed limit switch that can be used on all machines for the X axis. Machines with serial number 1688 and later came stock with this switch
J1-1
CAP+ 301
CAP- 300
PDB PDB +
8A
8A
15 A
8A
8A
DAUGHTERBOARD
FOR OPTIONAL PDB
8A
2A
8A
J1-48VAC L25
J2-48VAC L15
X+ 302
X- 303
Y+ 304
Y- 305
Z+ 306
Z- 307
A- 325
A+ 324
BRK+ 326
BRAKE RLY- 329
BRK- 327
BRAKE RLY+ 328
J1-2
J1-4
NOTE ORDER
OF WIRES
FROM T5 TO
B2 TO B4
OPTIONAL LOAD METER
(32096)
J1-6
J1-3
LM2
T1 to LM1 (J1-2)
B1 to LM2
400
401
402
L26
L16
ATC +
ATC -
403
404
STEPPER MOTORS TO STEPPER DRIVER
MOTOR
LEAD
COLOR
WIRE
NUMBER
DRIVER
TERMINAL
XYZ - 32000
A - 30467
RED
308
P2-3
X DRIVE
GRN
309
P2-4
X DRIVE
YEL
310
P2-5
X DRIVE
WIRE COLORS/GAUGE
WIRE
NUMBER
COLOR
SIZE
(AWG)
RED
312
P2-3
Y DRIVE
GRN
313
P2-4
Y DRIVE
100
WHITE
14/16
YEL
314
P2-5
Y DRIVE
101-199
RED
16
RED
316
P2-3
Z DRIVE
200
WHITE
16
GRN
317
P2-4
Z DRIVE
201
GREEN/YELLOW
16
YEL
318
P2-5
Z DRIVE
202-299
BLACK
16
RED
320
P2-3
A DRIVE
300-399
MULTI COLOR
16
WHITE
321
P2-4
A DRIVE
400-499
BLACK
14
YEL
322
P2-5
A DRIVE
J1-1 - J1-6
BLUE
18
GRN
323
P2-6
A DRIVE
L00-L99
BROWN/BLUE
14
White Wire
Black Wire 200
206
GRN/YEL Wire
Ground
White Wire
200
Black Wire
204 or 203
Green/Yellow Wire
Ground
X, Y, and Z Axis are Three Phase
A Axis (4th axis) is Bipolar
PIN 1
Connector
P1
P2
P3
P4
P5
Function
PWR GND
VDC
U
V
W
Connector
P1
P2
P3
P4
P5
P6
Function
PWR GND
VDC
A+
AB+
B-
PIN 1
PIN 1
SWITCH SETTINGS FOR
X, Y, Z
8" ROTARY TABLE
6" ROTARY TABLE
DETAILS: POT1 CONNECTIONS
1
2
2
POT1
3
3
POT1
1
SCHEMATIC (THEORY)
PHYSICAL
BACK SIDE VIEW
POT1 (PN 31041)
205
203
202
J3
204
202
POT1
CONNECTION BOARD
32089
OPERATOR PANEL with components identification
(32097)
OPERATOR PANEL with wire identification
BACK SIDE
Tools and Related Items
Number
Description
30409
Manual oil pump
31374
Automatic Oiler
31386
Machine Way Oil
30485
Spanner Wrench 25-28 mm -DIN 1804 applications, DIN 1810 form A standard. Used for setting
preload on ballscrew mount bearings. Two wrenches are needed
31118
Pin spanner, adjustable. 4 mm pins (for adjusting spindle bearing preload)
30527
Optical Tachometer 100,000 RPM laser optical tachometer. 5 digit digital display. Useful for
spindle speed calibration. Includes case.
32397
PCNC 1100 Manual: Replace your old manual with the latest version. Spiral bound. Manual
PDF can also be downloaded from www.tormach.com
30572
Touch Up Paint - Dark Gray 2.5 oz matching the lower section of the stand. Original paint is oil
based, touchup is latex.
30571
Touch Up Paint - Light Gray 2.5 oz matching the PCNC 1100 and the upper section of the stand.
Original paint is oil based, touchup is latex. We cannot ship paint during colder weather. NOTE:
Valspar Tractor and Implement paint #5339-13 Ford Gray is also a pretty close match.
30624
DIN connector - 5 pin. This is a plug that will fit in the accessory jack on the front of the machine
cabinet.
30482
CPC connector - reverse gender. This is the plug that is on the end of the 4th axis and connects
to the side of the PCNC cabinet.
30712
Machine Stand Door latch Left
30713
Machine Stand Door latch Right
30714
Machine Stand Door latch Center
30725
Coolant hose, armored
30508
Coolant Pump
31105
Coolant hose mount bracket
30726
Segmented spray hose (blue/orange)
31366
Coolant Refractometer
31101
Spindle Load Meter Top Mounted
32096
Spindle Load Meter Face Mounted
31706
Pneumatic Power Draw Bar
31728
Foot Pedal for Power Draw Bar
Appendices
10.3
Appendix 3 - Use of a Standard PC to control PCNC
You are strongly advised to use the Tormach Machine Controller to run the PCNC control
software. If you have a particular reason to attempt to use an standard PC running Windows XP
or Vista this appendix give some guidelines.
As such equipment is outsides Tormach’s control it will not be possible to offer detailed
support for its use.
10.3.1 Choice of computer
The system does not require a particularly powerful computer but there are certain requirements
for optimal operation. For Windows XP you should have:
•
A CPU running at least 1 GHz with at least 512 megabytes of RAM. Intel and AMD
processors are both satisfactory.
•
Video of 1024 x 768. Certain low cost computers with integrated video have shown
problems. In those situations the best solution is to disable the motherboard based video
and install an inexpensive video card in an expansion slot.
•
Laptop computers are unsuitable and, any which can be eventually be made to work,
will only do so by re-installing Windows without the APCI (Advanced Power
Configuration Interface). This will cripple the machine for normal portable use.
•
You need a parallel printer port (25 pin D socket). A USB to printer adaptor cannot be
used in place of this. If this port is on the motherboard then the standard configuration
will use it. PCI parallel ports from many manufacturers can, however, be used. You will
need to consult Chapter 9 for details of the configuration process for cards which do not
use the standard port address of 0x378.
•
Some motherboards based on the Via chipset have proved incompatible with the control
software. If you are buying such a board please ensure your supplier will take it back
and refund the cost in the unlikely event that you have problems.
•
A CD ROM or DVD drive is essential for software installation.
•
We advise you to use a USB storage device for transporting small files like G-code
programs to the machine tool. These devices are variously known as “flash,” “thumb,”
“jump” or “key” drives. The most common U.S. usage is “flash drive” and we will use
that from now on. Please note, G-code programs should not, however, be run directly
from the USB storage device. Transfer the G-code programs to the local hard disk,
remove the flash drive and run the program off the hard disk, not off the flash drive.
•
The computer can have network capability but it should not be used while the machine
tool is being used. In particular, Ethernet cards which will auto-negotiate to work at
10BaseT or 100BaseT should be set for a fixed speed or you will hear a “tick” from the
steppers every second or so during jogging as Windows takes control to negotiate
network speed. Do not run G-code programs off a network drive or remote computer.
•
Do not allow background automatic updates to be active while running the mill. Do not
leave Foxfire, Mozilla, Internet Explorer or Netscape run in the background while
operating the mill.
There are some features in the computer that will make operation of the PCNC more
convenient. Things to look for are:
•
A computer which will boot-up when it sees AC power switched on – rather than
needing you to press a button. This feature generally is controlled by a BIOS option and
can be enabled by entering the BIOS configuration mode.
•
A keyboard that includes a small USB hub to plug in a USB flash drive for loading part
programs. Connect all other USB devices directly to the PC motherboard.
Using Tormach PCNC 1100 Series 3
10-14
32397 Rev C1-2
Appendices
Modern multi-core high performance computers are less likely to work well than older more
modest performers. The chip makers now employ a variety of power saving techniques which
compromise real-time performance.
10.3.2 Optimizing the Windows Installation
It is important that the computer used to control your PCNC does not have a large load of
software running in the background. Examples are the automatic update utilities for Windows
and virus/spam checkers, Multimedia software and telephony and messaging software. Such
software can wake up at any time and place large loads on the computer and its disk subsystem. This can sometimes interfere with timing of movement of PCNC and lead to spoiled
work.
The simplest advice is:
•
If you are using an existing computer that has been used for some time there are likely
to be a number of unnecessary programs or drivers loaded when the computer boots.
Windows can be hard to “clean up,” the best solution is often to re-install Windows after
formatting the hard drive. You may prefer to ask an IT specialist to help you with this.
•
Install the minimum options for Windows. You should include access to the Internet so
you can maintain your system software and access the Tormach web site but you will
normally run with the network disabled.
•
Do not install other software packages on the computer. If you wish the control
computer to be dual purpose then we advise you to create two partitions on the hard
drive. Install Windows in both but keep one as the minimal installation for the control
software for the PCNC. The other partition can contain what you like. When you switch
on you can choose from which partition you want to boot.
The section below gives a checklist of actions to achieve the “leanest” Windows system. The
recommendations there are helpful, but not always necessary. Do not leap in and do everything
unless you have problems with machine motion. Apply them in the order given until jogging
and rapid moves are smooth. Optimization of Windows is more important on slower computers
(below 1.6 GHz).
10.3.3 Installing the Control Software
10.3.3.1 Installing
You do not need the PCNC connected to the computer by the parallel cable yet. If you are just
starting it would be better not to have it connected. You must not have a printer connected to
the parallel port. The Control Software will not operate correctly with a printer attached to the
parallel port and it may damage the printer. Switch off the PC, the PCNC and unplug the 25 pin
connector from the back of the PC. Now switch the PC back on.
Load the release CD into your CD drive. If you have “auto run” configured on your computer
then the installer will start running.
Otherwise use Windows Explorer or the My Computer icon to open the CD. Select
View>Details from the menu. Double-click on the file Install.BAT to run it. You will be guided
through the usual installation steps for a Windows program such as accepting the license
conditions and selecting the folder for the control software. Accept all the defaults. You will
now be told to reboot before running the Control Software.
Your installation will come with a second CD which contains your license file. Follow the
instructions to put a copy of your numbered license file and the working license into the PCNC
folder. This stage is most important or you will not be able to run programs longer than about
500 lines and various features are disabled.
32397 Rev C1-2
10-15
Using Tormach PCNC 1100 Series 3
Appendices
10.3.3.2 Vital Re-boot
After you have initially installed the Control Software program, you must re-boot your
computer. This reboot is vital. If you do not do it then you will get into great difficulties which
can only be overcome by using the Windows Control Panel to uninstall the driver manually. So
please reboot now.
If you are interested in knowing why the reboot is required then read on, otherwise skip to the
next section.
Although the Control Software will appear to be a single program when you are using it, it
actually consists of two parts; a driver which is installed as part of Windows like a printer or
network driver and a graphical user interface (GUI). The reasons for this division are complex
but the driver is the most important and ingenious part.
The Control Software must be able to send very accurately timed signals to control the axes of
the machine tool. Windows likes to be in charge and runs normal user programs when it has
nothing better to do itself. So the Control Software cannot be a “normal user program;” it must
be at the lowest level (highest priority in the computer) inside Windows (that is, it handles
interrupts). Furthermore to do this at the high speeds possibly required (each axis is given
attention 25,000 times per second) the driver needs to tune its own code. Windows does not
approve of this (viruses often play this trick) so it has to be asked to give special permission.
This process requires the reboot. So if you have not done the re-boot then Windows will give
the Blue Screen of Death and the driver will be corrupt. The only way out of this will be to
manually remove the driver.
Having given these dire warnings, it is only fair to say that, although requested when upgrades
are installed, the reboot is only strictly required when the driver is first installed. Windows XP
boots reasonably quickly that it is not much hardship to do it every time.
10.3.3.3 Testing the Installation
It is now highly recommended to test the system. The Control Software is not a simple
program. It takes great liberties with Windows in order to perform its job in fact it actually runs
Windows rather than Windows running it; this means it will not work on all systems due to
many factors. For example, QuickTime’s system monitor (qtask.exe) running in the background
can kill it and there will be other programs which you probably are not even aware are on your
system that can do the same. Windows can and does start many processes in the background;
some appear as icons in the systray and others do not show themselves in any way. Other
possible sources of erratic operation are local area network connections which may be
configured to automatically speed detect. You should configure these to the actual speed 10
Mbps or 100 Mbps of your network.
Because of these factors, it is
important that you test your
system when you suspect
something is wrong or you
just want to check that the
install went well.
Navigate by Windows
Explorer to the PCNC folder
(usually C:\PCNC3). Double
click the file DriverTest or if
you display file extensions
DriverTest.exe (figure A3.1).
Figure A3.1 – The DriverTest program display
You can ignore all the boxes
with the exception of the
Pulse Frequency. It should be
fairly steady around
Using Tormach PCNC 1100 Series 3
10-16
32397 Rev C1-2
Appendices
24,600Hz, but may vary, even wildly, on some systems. This does not necessarily mean the
pulse timer is unsteady, it may mean that the computer is heavily loaded or slow to begin with,
since the Control Software takes the highest priority in the system, the clock may be shunted
down to a priority slow enough that its one second is a variable length of time. Since the pulse
count is based on one second of Windows time, variations in Windows time will make the pulse
count look like it is swinging around a lot even when it is rock solid. Basically, if you see a
similar screen to figure A3.1, everything is working well so close the DriverTest program
and skip to the section Running the PCNC below.
Windows “experts” might be interested to see a few other things. The white rectangular
window is a type of timing analyzer. When it is running it displays a line with small variations
indicated. These variations are the changes in timing from one interrupt cycle to another. There
should be no lines longer than 1/4" or so on an 17" screen on most systems. Even if there are
variations its possible they are below the threshold necessary to create timing jitters so when
your machine tool is connected you should perform a movement test to see if jogging and
G00/G01 moves are smooth. A line with big spikes or other patterns will limit the high speed
performance of your mill.
You may have one of three things happen to you when running the test which may indicate a
problem.
1. Screen shows wide variation or clearly periodic variation of timing. In this case you need to
complete a computer optimization detailed in Appendix 3 (section 10.3 of this manual).
2. “Driver not found or installed, contact Art.” This means that the driver is not loaded into
Windows for some reason. This can occur on XP systems which have a corruption of their
driver database, reloading Windows is the cure in this case.
3. When the system says, taking over…3…2…1... and then reboots, one of two things has
occurred. Either you did not reboot when asked (told you!!) or the driver is corrupted or
unable to be used in your system. In this case follow the next section and remove the driver
manually, then re-install. If the same thing happens, please notify Tormach by e-mail and
you will be given guidance. A few systems have motherboards which have hardware for an
APIC timer but whose BIOS code does not use it. This will confuse the Control Software
install. A DOS batch file “specialdriver.bat” to run in a DOS window is available; this will
make the driver use the older i8529 interrupt controller. To display the DOS window enter
CMD as the program after Start Button>Run. You will need to repeat this process
whenever you download an upgraded version of the Control Software as installing the new
version will replace the special driver.
10.3.3.4 DriverTest After a Software Crash
Should you for any reason have a situation when the Control Software crashes – this might be
an intermittent hardware problem or software bug – then you must run DriverTest as soon as
possible after the Control Software has failed. If you delay for two minutes then the Control
Software driver will cause Windows to fail with the usual Blue Screen of Death. Running
DriverTest resets the driver to a stable condition even if the rest of the Control Software
disappears unexpectedly. If you have a troublesome system then you might find it worthwhile
to create a shortcut for DiverTest.exe and drag it onto the Desktop for easy access.
10.3.3.5 Manual Driver Installation and Un-installation
You only need to read and do this section if you have not successfully run the DriverTest
program.
The driver (Mach3.sys) can be installed and uninstalled manually using the Windows control
panel.
•
32397 Rev C1-2
Open the Windows Control Panel and double-click on the icon or line for System.
10-17
Using Tormach PCNC 1100 Series 3
Appendices
•
Select Hardware and click Add Hardware wizard. As mentioned before the Control
Software’s driver works at the lowest level in Windows. Windows will look for any new
actual hardware (and find none).
•
Tell the wizard you have already installed it and then proceed to the next screen.
•
You will be shown a list of hardware. Scroll to the bottom of this and select Add a new
hardware device and move to the next screen.
•
On the next screen you do not want Windows to search for the driver so select Install the
hardware that I manually select from a list (Advanced).
•
The list you are shown will include an entry for Mach x pulsing engine. Select this and
go to the next screen.
•
Click Have disk and on the next screen point the file selector to your directory
(C:\PCNC3 by default). Windows should find the file Mach3.inf. Select this file and
click Open. Windows will install the driver.
The driver can be uninstalled rather more simply.
•
Open the Control panel and double-click on the icon or line for System.
•
Select Hardware and click Device Manager.
•
You will be shown a list of devices and their drivers. Mach x Pulsing Engine has the
driver Mach3 Driver under it. Use the + to expand the tree if necessary. Right-click on
Mach3 Driver gives the option to uninstall it. This will remove the file Mach3.sys from
the Windows folder. The copy in the PCNC3 folder will still be there.
10.3.4 Optimization of Windows XP
The PC running your mill does not simply send G- & M-codes down to the mill; rather it is
intimately involved with control of the axis motors and spindle. It reviews and updates
electrical signals to every axis motor 25,000 times each second. If your PC is busy thinking
about other things, there can be problems in motion control.
We advise you not to cut a part with the control computer connected to a network.
Note: If you have a computer supplied by Tormach as part of your mill package then you do
not need to perform the steps in this section.
The steps listed below
will optimize
Windows XP. There
are a large number of
esoteric Windows
functions which, if
enabled, can cause
problems. You will
know if you have
difficulties if machine
motion sounds rough
or if a long move
makes a periodic
ticking sound.
In difficult cases
please consult
Tormach for more
detail changes that could be made.
Using Tormach PCNC 1100 Series 3
Figure A3.2 – Disable Startup programs
10-18
32397 Rev C1-2
Appendices
10.3.4.1 Remove Unnecessary Services and Startup Programs
Background: There are a variety of programs that can run in the background, stealing CPU
power. These programs may watch your keystrokes, track communications or try to seek out
networks. New
computers are often
laden with “freebee”
versions of programs
that are loaded when
the computer starts.
Things to remove
include QuickTime,
RealPlayer, AOL
messenger,
QuickBooks, Instant
Messenger, camera,
video software, music
software and just about
any application
software that you do
Figure A3.3 – Disable Services
not use or recognize.
Your mill computer
should be lean and clean and void of any unnecessary programs.
1.
2.
3.
4.
5.
Click Start button.
Click Run.
Type MSCONFIG and press Enter.
Click Services tab.
On the lower line, check the box for Hide All Microsoft Services (step 1), then Disable All
(step 2), finally click on Apply (step 3)
6. Now click on the Startup tab
7. Click on Disable All then Apply. Some people prefer to have the PCNC software called out
in the Startup group so the control program is running as soon as the computer is turned on.
In this case leave that as the only Startup program.
8. Click OK to complete.
10.3.4.2 Disable Power Management
1. Right-click on your desktop and then click Properties.
2. Click on the Screen Saver tab.
3. Set Screensaver to None.
4. Press the Power button near the bottom.
5. Set all options to NEVER shut down automatically!
10.3.4.3 Disable sound card
Background: The Control Software emits a Beep sound when it executes a G-code commen
(i.e. text in round brackets). Some sound cards inhibit interrupts and can cause lost steps when
doing this. The trouble can happen even if no speakers are attached to the computer.
•
Open the Control panel and double-click on the icon or line for System.
•
Select Hardware and click Device Manager.
•
You will be shown a list of devices and their drivers. Locate Sound, Video and Game
controllers. Use the + to expand the tree if necessary. Right-click on any driver gives
32397 Rev C1-2
10-19
Using Tormach PCNC 1100 Series 3
Appendices
the option to Disable it. Do this for all sound devices on the system – there will usually
only be one.
10.3.4.4 Disable Automatic Updates
Background: Automatic updates can initiate a CPU stealing background task. This can create
havoc if it occurs while the machine is running a program. Some updates force a system re-boot
after a timeout period. This is disastrous when running a job with the screen unattended.
1. Right Click My Computer and select Properties.
2. Click Automatic Updates tab.
3. Uncheck Keep my computer updated.
4. Click OK.
10.3.4.5 Set Computer to Standard PC not ACPI PC
Background: This optimization procedure is not needed on most computers, but it is required
on some. We recommend this procedure only be applied last and only if necessary. Advanced
Configuration and Power Interface) is a power management specification that allows the
operating system to control the how power is applied to the computer’s devices. For example,
an ACPI PC can be turned off completely by using Windows Shutdown function. With a
Standard PC (not ACPI), the Windows Shutdown function will close programs and prepare the
operating system, then open a window with the statement "You can now turn off your
computer". A Standard PC can only be turned off at the power switch on the box itself, not
through the operating system.
1. Right Click My Computer and select Properties.
2. Click Hardware tab.
3. Click Device Manager button in the middle.
4. Double click Computer.
5. Right click on Standard ACPI PC and choose Update Driver.
6. Choose Install the software from a Specific Location (Advanced).
7. Click Next.
8. Choose Do not search. I will choose driver to install.
9. Click Next.
10. Choose Standard PC from the listing.
11. Click Next.
12. Click OK.
When you re-boot Windows will have to find and load many drivers. The Standard PC drivers
for the video, hard disk, keyboard and other devices are all different than the ACPI drivers. This
can take a long time and it may appear to have frozen for many minutes during the process. It
may require re-booting several times.
Using Tormach PCNC 1100 Series 3
10-20
32397 Rev C1-2
Appendices
10.4
Revision history
Rev C1-2
22 September
2011
Initial release of Series 3 manual
Rev B1-4
12 August 2011
Clarification of details, correction of minor errors and
reference to updated products supporting the mill.
Rev C4-2
10 Sept 2008
This version of PCNC Series I is base manual for this
documentation
32397 Rev C1-2
10-21
Using Tormach PCNC 1100 Series 3
Appendices
11.
Index
Hint: Where there is a choice, most index entries are made using the name of a thing (e.g.,
tool offset) rather than an action (e.g., measuring) so you will get better results thinking
about the part of the machine on which you want information. Thus looking for “Tool offset
– measuring” will give better results than looking for “Measuring – tool offset.” For
important information both entries will probably appear.
If you have difficulty because you tried to look something up and the index entry
was missing, please take a moment to e-mail [email protected] with a note of
(a) the words you were looking up and (b) where in the manual you found the
information you wanted – assuming you did!
Block
format of code .................................................7-5
Block Delete
action of ..........................................................7-4
Block delete switch ............................................ 5-11
Blue Screen of Death
action to avoid ............................................. 10-17
Boring and reaming canned cycle
G85 ............................................................... 7-30
Boring manual retract canned cycle
G88 ............................................................... 7-30
Boring with dwell and retract canned cycle
G89 ............................................................... 7-30
Boring with dwell canned cycle
G86 ............................................................... 7-30
A
Absolute distance mode
G90 ............................................................... 7-30
Absolute IJ mode ............................................... 7-16
Absolute machine coordinates
G53 - move in ............................................... 7-24
Accessory socket ............................................... 2-12
on control panel ...............................................5-2
Address
setting non-stsetting non-standard printer port 9-13
Adjustable parallel gauge .....................................6-8
Arc - center format............................................. 7-16
Arc - radius format............................................. 7-15
Arc at feedrate
G02/G03 defined ........................................... 7-15
Arc motion
defined ............................................................7-2
Assemply Y-axis drive .........................................2-4
Axis controls family
described .........................................................5-6
Axis coordinate DRO
described .........................................................5-6
Axis jogging
control family
described .....................................................5-8
keyboard
Continuous ..................................................5-8
Step.............................................................5-8
MPG ...............................................................5-8
rate override ....................................................5-8
Step selected by Ctrl key..................................5-8
with Tormach Jog/Shuttle Controller................5-8
C
Cabinet/stand .......................................................2-5
CAD
2d, 2 ½D and 3D explained..............................4-2
CAD/CAM software
what to look for ...............................................4-2
Calculator
feeds ans speeds ............................................ 5-15
Cancel modal motion
G80 explained ............................................... 7-26
Canned cycle return level
G98/G99 ....................................................... 7-32
Canned cycles .................................................... 7-26
in-between motion ......................................... 7-28
preliminary motion ........................................ 7-28
repeats by L word .......................................... 7-27
retract defined by R word............................... 7-27
sticky numbers .............................................. 7-27
Center format arc ............................................... 7-16
Centering microscope methods........................... 6-12
Circular pocket
G12/G13 ....................................................... 7-18
Code definition syntax explained ....................... 7-11
Column and head assembly ................................ 10-1
B
Base assembly - exploded view .......................... 10-3
Bearings, ballscrew
adjustment of preload ......................................9-8
Binary operations
defined ............................................................7-8
32397 Rev C1-2
23
Using Tormach PCNC 1100 Series 3
Index
Direction of jogging........................................... 2-14
Display mode button .......................................... 5-12
Diver test program ........................................... 10-16
Drilling canned cycle
G81 ............................................................... 7-28
Drilling with dwell canned cycle
G82 ............................................................... 7-29
Dwell ..................................................................7-3
G04 - defined ................................................ 7-17
Comments
defined ............................................................7-9
Computer LED
on control panel ...............................................5-2
Computer mounting
accessories ......................................................2-3
arrangements ...................................................2-3
Computer ON/OFF
control panel switch ................................ 2-11, 5-2
Computer requirements ........................................2-8
Concept behind PCNC .........................................1-3
Connecting control computer to PCNC............... 2-10
Constant velocity mode
G64 - setting.................................................. 7-25
purpose of explained........................................7-3
Control panel controls explained ........................ 2-10
Control power
troubleshooting.............................................. 9-28
Control Software
Components of ............................................ 10-16
screens ............................................................5-5
Controlled point
defined ............................................................7-2
Conversationl programming .................................4-9
Coolant
control of.........................................................7-3
control panel switch ....................................... 2-12
importance of in CNC......................................2-2
M07 - mist on ................................................ 7-34
M08 - flood on .............................................. 7-34
M09 - all off .................................................. 7-34
Coolant controls
on control panel ...............................................5-2
Coordinate rotation by probing
setting coordinate rotation .............................. 8-11
Coordinate system rotation
G68 – setting and G68 - clearing .................... 7-25
Coordinate systems
and offsets .......................................................6-1
reference definitions ........................................7-5
Co-ordinated linear motion
defined ............................................................7-2
Current position
defined ............................................................7-3
Cutter compensation
tool diameter
entry move
general .................................................. 6-19
Cutter diameter compensation
through CAD/CAM ....................................... 6-15
Cutter radius compensation
G40/G41/G42 defined ................................... 7-23
Cycle Start button .............................................. 5-10
E
Electrical overview diagram ............................... 10-5
Electrical specifications .......................................9-2
EStop button ...................................................... 2-11
on control panel ...............................................5-2
Exact stop mode
G61 - setting.................................................. 7-25
purpose of explained........................................7-3
Excecution of words
order of ......................................................... 7-37
Exploded view
base assembly................................................ 10-3
column and head assembly............................. 10-1
Expressions
defined ............................................................7-8
F
F word -feedrate ................................................ 7-36
Feed & Speed calculator .................................... 5-15
Feed and speed override
controlled by M48/M49 ................................. 7-34
Feedrate
defined ............................................................7-2
display DROs
described ................................................... 5-10
F word to set.................................................. 7-36
inverse time - G93 ......................................... 7-31
units per minute - G94 ................................... 7-31
units per rev.....................................................5-9
units per rev - G95 ......................................... 7-31
Feedrate control family
described .........................................................5-9
Feedrate units per rev - G95 ............................... 7-31
File control family ............................................. 5-12
First part
making ............................................................3-1
Fixture coordinate select
G54-G59 defined ........................................... 7-24
Fixture coordinate systems - setting - G10 .......... 7-18
Fourth axis
diameter compensation of feedrate ...................8-1
engraving on a cylinder....................................8-2
gear cutting .....................................................8-3
referencing and zeroing ...................................8-1
Fourth axis on PCNC ...........................................8-1
Frequently Found Problems ............................... 9-21
From idea to a part ...............................................4-1
D
Demonstration program
running............................................................3-2
Diameter compensation LED
described .........................................................5-7
Digitizer probe .....................................................8-4
Digitizer probe interface .................................... 8-13
Using Tormach PCNC 1100 Series 3
G
G & M codes
overview .........................................................4-1
24
32397 Rev C1-2
Appendices
G99 - canned cycle return level
to R word ...................................................... 7-32
G-code
running............................................................4-6
G-code display control ....................................... 5-11
G-codes
summary table ............................................... 7-12
Goto toolchange ................................................ 5-11
G00 - rapid linear motion ................................... 7-13
G01 - linear feedrate move ................................. 7-13
G02 - clockwise arc ........................................... 7-15
G03 - counterclockwise arc ................................ 7-15
G04 - dwell........................................................ 7-17
G10 - set coordinate systems .............................. 7-18
G12 - circular pocket ......................................... 7-18
G13 - circular pocket ......................................... 7-18
G15 - exit Polar mode ........................................ 7-18
G16 - enter Polar mode ...................................... 7-18
G17 - select XY plane ........................................ 7-19
G18 - select XZ plane ........................................ 7-19
G19 - select YZ plane ........................................ 7-19
G20 - inch units - setting .................................... 7-19
G21 - millimetre units - setting........................... 7-19
G28 - return to home.......................................... 7-20
G28.1 - reference axes ....................................... 7-20
G30 - return to home.......................................... 7-20
G31 - and probe hardware options ........................8-5
G31 - straight probe ........................................... 7-20
G40 - cutter radius compensation - Off ............... 7-23
G41 - cutter radius compensation - Left .............. 7-23
G42 - cutter radius compensation - Right............ 7-23
G43 - enable tool length offset ........................... 7-23
G44 - enable tool length offset ........................... 7-23
G49 - disable tool length offset .......................... 7-23
G50 - clear axis scale factors .............................. 7-23
G51 - set axis scale factors ................................. 7-23
G52 offsets ........................................................ 7-24
G53 - move in absolute machine coordinates ...... 7-24
G54 - select fixture 1 ......................................... 7-24
G55 - select fixture 2 ......................................... 7-24
G56 - select fixture 3 ......................................... 7-24
G57 - select fixture 4 ......................................... 7-24
G58 - select fixture 5 ......................................... 7-24
G59 - select any fixture ...................................... 7-24
G61 - set exact stop mode .................................. 7-25
G64 - set constant velocity mode ........................ 7-25
G68
define coordinate system rotation ................... 7-25
G69
Clear coordinate system rotation .................... 7-25
G73
- high speed peck drilling canned cycle .......... 7-26
pullback DRO ............................................... 7-26
G80 - cancel modal motion ................................ 7-26
G81 - drilling canned cycle ................................ 7-28
G82 - drilling with dwell canned cycle ............... 7-29
G83 - peck drilling canned cycle ........................ 7-29
G85 - boring and reaming canned cycle .............. 7-30
G86 - boring with dwell canned cycle ................ 7-30
G88 - boring manual retract canned cycle ........... 7-30
G89 - boring with dwell and retract cycle ........... 7-30
G90 - absolute distance mode............................. 7-30
G91 - incremental distance mode ....................... 7-30
G92 - workpiece offsets
interaction with parameters ............................ 7-31
G92 offsets ........................................................ 7-31
G93 - feedrate inverse time ................................ 7-31
G94 - feedrate units per minute .......................... 7-31
G98 - canned cycle return level
to old Z ......................................................... 7-32
32397 Rev C1-2
H
Home - return to G28/G30 ................................. 7-20
I
I/J Modes setting................................................ 5-16
IJ mode - "Absolute".......................................... 7-16
IJ mode - Increments.......................................... 7-16
Inch units
G20 - setting.................................................. 7-19
Incremental distance mode
G91 ............................................................... 7-30
Incremental IJ mode........................................... 7-16
Inhibits and overrides control family .................. 5-15
Installation
errors after ................................................... 10-17
of control software....................................... 10-15
of driver
manual .................................................... 10-17
Intelligent labels
described .........................................................5-6
Intended use
policy if use is out of scope ..............................9-1
statement of .....................................................9-1
Isolator ......................................... See - Main switch
J
Jerky motion with short lines
Constant velofity mode to avoid .......................7-3
Jog/Shuttle controller ...........................................5-8
Jogging
direction of .................................................... 2-14
Jogging axes ...................................................... 2-14
Jogging pendant ................................................. 5-16
L
Laser finder methods ......................................... 6-12
Learning and Training..........................................2-3
Lifting onto stand ................................................2-5
Lighting for machine ...........................................2-2
Line
format of code .................................................7-5
Line DRO
described ...................................................... 5-11
Line number
format of .........................................................7-7
Linear axes
defined ............................................................7-1
Linear feedrate move
G01 defined................................................... 7-13
Location of machine ............................................2-1
Location to give safety .........................................2-2
Locking
25
Using Tormach PCNC 1100 Series 3
Index
spindle.............................................................5-3
Loop control family ........................................... 5-13
N
Number
format of .........................................................7-7
M
M00 - program stop ........................................... 7-32
M01 - optional program stop .............................. 7-32
M02 - program end ............................................ 7-32
M03 - spindle clockwise .................................... 7-33
M04 - spindle counterclockwise ......................... 7-33
M05 - stop spindle ............................................. 7-33
M07 - mist coolant on ........................................ 7-34
M08 - flood coolant on....................................... 7-34
M09 - all coolant off .......................................... 7-34
M30 - program end ............................................ 7-32
M48 - feed and speed override on....................... 7-34
M49 - feed and speed override off ...................... 7-34
M871
tapping canned cycles .................................... 7-35
M87x
tapping canned cycles .................................... 7-35
M98 - subroutine call ......................................... 7-34
M99 - subroutine return ..................................... 7-34
Mach license installation ......................................2-9
Machine coordinates
G53 - move in ............................................... 7-24
Machine modes
defined .......................................................... 7-10
Machine ON LED.............................................. 2-11
MachOS ..............................................................2-9
Macro M-codes.................................................. 7-35
Macros
overview on writing....................................... 7-35
Main switch ................................................ 2-10, 5-1
Maintenance
Bearing preload adjustment..............................9-8
lubrication .......................................................9-5
protection from rust .........................................9-5
speed calibration ............................................ 9-11
way covers ......................................................9-6
Manual Data Input to control Software ............... 2-14
M-code
macros........................................................... 7-35
M-codes - built in
summary table ............................................... 7-32
MDI .................................................................. 2-14
Mechanical specifications ....................................9-2
Messages
from part program, defined ..............................7-9
Millimetre units
G21 - setting.................................................. 7-19
Mirroring parts ....................................................7-1
Modal groups
defined .......................................................... 7-10
Modal motion, cancelling
G80 explained ............................................... 7-26
Mode
of jogging ...................................................... 2-14
Modes
machine - defined .......................................... 7-10
MSG,
string introduces an operator message ..............7-9
Using Tormach PCNC 1100 Series 3
O
Offsets
G52 ............................................................... 7-24
G92 ............................................................... 7-31
Offsets and coordinate systems ............................6-1
Operators - binary
defined ............................................................7-8
Operators - unary
defined ............................................................7-8
Operator's panel ...................................................5-1
Optimising Windows ....................................... 10-15
Optimising Windows for PCNC ....................... 10-18
Optional program stop
M01 .............................................................. 7-32
Optional Stop
action of ..........................................................7-4
Optional Stop switch.......................................... 5-11
Order of G-code items on line ..............................7-9
Override
for feed and speed - disabling...........................7-4
Override feed and speed
controlled by M48/M49 ................................. 7-34
P
Parameter
setting value of ................................................7-9
using value of ..................................................7-7
Parameters
predefined .......................................................7-5
Part program
repeating indefinitely - M47........................... 7-34
repeating indefinitely -M99............................ 7-34
running controls family
described ................................................... 5-10
Part-program
making with Wizards .......................................4-9
Pause button ...................................................... 5-11
PCNC
choosing location of.........................................2-1
computer requirements ....................................2-8
connecting to control computer ...................... 2-10
control panel....................................................5-1
control panel controls explained ..................... 2-10
fourth axis option.............................................8-1
operator's panel................................................5-1
receiving and unpacking ..................................2-4
tool changing...................................................5-3
PCNC computer mounting arrangements..............2-3
PCNC concept .....................................................1-3
PCNCConfig
Defining Probe type ....................................... 9-15
Peck drilling canned cycle
G83 ............................................................... 7-29
Peck drilling canned cycle – high speed
G73 ............................................................... 7-26
Pendant - jogging............................................... 5-16
26
32397 Rev C1-2
Appendices
Return level after canned cycle
G98/G99 ....................................................... 7-32
Rewind button ................................................... 5-10
Roller gauge ........................................................6-7
Roll-you-own gauge ............................................6-7
Rotational axes
defined ............................................................7-1
Rotational diameter correction
controls family .............................................. 5-14
Run from here button ......................................... 5-11
Performance expectations ....................................1-3
Plane selection
G17/G18/G19 defined ................................... 7-19
Polar mode ........................................................ 7-18
Power distribution
troubleshooting.............................................. 9-24
Power supply requirements ........................... 2-3, 2-7
Preface ................................................................1-1
Printer port
setting non-standard address .......................... 9-13
Probe ............................................ See Straight probe
calibration ..................................................... 8-12
Probes and Tool setters ........................................8-4
Probing
comprehensive X/Y .........................................8-9
finding center of bore.......................................8-6
finding position of a face .................................8-6
for corner of a vise...........................................8-6
setting coordinate rotation .............................. 8-11
simple X/Y ......................................................8-5
surface Z .........................................................8-8
Z axis ..............................................................8-7
Profile
display name of profile in use ..........................5-6
Program
error handling ................................................ 7-37
Program end
M02/M30 ...................................................... 7-32
Program extrema ............................................... 5-12
Program stop
M00 .............................................................. 7-32
Pullback DRO
G73 ............................................................... 7-26
Pulleys
spindle speed control
described .....................................................5-9
S
S word - spindle speed ....................................... 7-36
Safety
checklist ..........................................................1-2
Dual supply - implications of ...........................1-1
from machine location and mounting ...............2-2
further reading .................................................1-2
general ............................................................1-1
Grounding .......................................................1-1
Safety warning.....................................................1-1
professional advice ..........................................1-1
Scale factor - on axis data - G50, G51 ................ 7-23
Scale factor DRO
described .........................................................5-7
Scaling coordinates ..............................................7-1
Scaling parts ........................................................7-1
Screen switching buttons......................................5-6
Screen switching controls
described .........................................................5-6
Selected plane
defined ............................................................7-3
Set fixture coordinate systems - G10 .................. 7-18
Set next line button ............................................ 5-11
Shuttle controller .................................................5-8
Simulate Program Run button ............................ 5-12
Single button ..................................................... 5-10
Space required - minimum ...................................2-2
Special Mach3.sys driver
installation of............................................... 10-17
need for ....................................................... 10-17
specialdriver.bat............................................... 10-17
Specification
options ............................................................9-3
Specifications
electrical..........................................................9-2
mechanical ......................................................9-2
system .............................................................9-3
Speed and feed override
controlled by M48/M49 ................................. 7-34
Spindle
belt changing ...................................................5-5
Changing the belt position ............................. 2-12
Control panel Forward/Reverse switch .........2-12
Control panel Start switch .............................. 2-12
Control panel Stop switch .............................. 2-12
locking ............................................................5-3
Lockout switch .............................................. 2-12
M03 - clockwise ............................................ 7-33
M04 - counterclockwise ................................. 7-33
M05 - stop ..................................................... 7-33
R
R8 tooling
inserting and removing ....................................5-3
Radius format arc............................................... 7-15
Rapid motion
G00 definrd ................................................... 7-13
Reaming and boring canned cycle
G85 ............................................................... 7-30
Re-boot during installation
how to manually uninstall driver if you fail to do it
............................................................... 10-18
reason for .................................................... 10-16
Receiving new machine .......................................2-4
Reference - G28.1.............................................. 7-20
Referenced LED
described .........................................................5-6
Referencing
importance of ..................................................3-2
introduction to .................................................3-1
Regen button ..................................................... 5-12
Repeating part program indefinitely - M47 ......... 7-34
Repeating part program indefinitely - M99 ......... 7-34
Reset button
described .........................................................5-6
32397 Rev C1-2
27
Using Tormach PCNC 1100 Series 3
Index
Tormach Jog/Shuttle controller ............................5-8
Tormach Machine Controller ...............................2-8
Tormach Tooling System
TTS.................................................................5-3
Touching techniques ............................................6-6
Transportation of machine ................................. 9-57
Troubleshooting
axis drive sub-system ..................................... 9-33
computer control communications ................. 9-31
control power ................................................ 9-28
electrical........................................................ 9-57
Frequently Found Problems ........................... 9-21
mechanical .................................................... 9-56
overview ....................................................... 9-16
philosophy..................................................... 9-16
power distribution.......................................... 9-24
spindle drive sub-system ................................ 9-48
tools .............................................................. 9-20
TTS - Tormach Tooling System ...........................5-3
TTS tooling
inserting and removing ....................................5-4
Typographics conventions in this manual .................
Manual/Auto ................................................. 2-12
Spindle controls
on control panel ...............................................5-2
Spindle speed
control family described ..................................5-9
S word to set.................................................. 7-36
Spindle speed calibration ................................... 9-11
Stand/cabinet .......................................................2-5
Start button ........................................................ 2-11
on control panel ...............................................5-2
Status LEDs
on control panel ...............................................5-2
Step size
customizing the standard list .......................... 9-14
Stop button ........................................................ 5-10
Straight probe
example program ........................................... 7-21
G31 defined.............................. See Straight probe
Subroutine call
M98 .............................................................. 7-34
repeating several times................................... 7-34
Subroutine label
format of .........................................................7-7
Subroutine return
M99 .............................................................. 7-34
Support
from Tormach .................................................9-1
Switch - main .................................................... 2-10
Syntax - Code definition .................................... 7-11
System specifications...........................................9-3
1-5
U
Unary operators
defined ............................................................7-8
Un-installation of driver
manual ........................................................ 10-18
Units
inch, degree ans millimetre ..............................7-3
Unpacking new machine ......................................2-4
Unusual modes
when Control Software is running .................. 5-13
T
T word - tool select ............................................ 7-36
Tapping
Dwell mode - for blind holes.......................... 8-16
sequence for threading a hole ......................... 8-15
Tapping heads
description of the heads ................................. 8-14
Teach control family .......................................... 5-12
Testing
Control Software installation ....................... 10-16
DiverTest program....................................... 10-16
Tool change
supplied M6 macros....................................... 7-33
Tool change position
going to ......................................................... 7-35
Tool changing......................................................5-3
Tool length
setting by tool setter.........................................8-8
Tool length offset
G43 - enable .................................................. 7-23
G44 - enable .................................................. 7-23
G49 - disable ................................................. 7-23
Tool select
T word .......................................................... 7-36
Tool setters and probes ........................................8-4
Toolchange position control family .................... 5-14
Toolpath
display looks inaccurate ................................. 5-12
Using Tormach PCNC 1100 Series 3
W
Windows
optimisation procedures ............................... 10-18
Wizard
checking code output by ................................ 4-10
Wizards
for conversational programming ......................4-9
Word
format of .........................................................7-7
intial letters .....................................................7-7
Work offsets
by Touch buttons .............................................6-9
by typing into DRO .........................................6-9
setting X and Y by probe ............................... 6-11
using more than one....................................... 6-14
X
XMLTweak
setting non-standard address .......................... 9-13
spindle speed calibration ................................ 9-11
Y
Y-axis drive
assembling on new machine.............................2-4
28
32397 Rev C1-2
Was this manual useful for you? yes no
Thank you for your participation!

* Your assessment is very important for improving the work of artificial intelligence, which forms the content of this project

Download PDF

advertisement