prototrak Bed Programming Manual

Service Department: 800.367.3165

TRAK

ProtoTRAK

Safety, Programming, Operating and Care Manual

Covers Models:

TRAK DPMSX2

® Bed Mills

® SMX CNC

Document: 24495
Version: 042913

TRAK DPMSX3
TRAK DPMSX5
TRAK FHM5
TRAK FHM7

Southwestern Industries, Inc.

2615 Homestead Place
Rancho Dominguez, CA 90220-5610 USA
T | 310.608.4422 | F | 310. 764.2668

e-mail: sales@southwe sterni ndustrie s.com | [e-mail] | web:
southwesternindustries.com

Copyright © 2012, Southwestern Industries, Inc. All rights are reserved. No part of this
publication may be reproduced, stored in a retrieval system, or transmitted, in any form or by any
means, mechanical, photocopying, recording or otherwise, without the prior written permission of
Southwestern Industrie s, Inc.

While every effort has been made to include all the information required for the purposes of this
guide, Southwestern Industries, Inc. assumes no responsibility for inaccuracies or omission and
accepts no liability for damages resulting from the use of the information contained in this guide.

All brand names and products are trademarks or registered trademarks of their respective
holders.

Southwestern Industries, Inc.
2615 Homestead Place
Rancho Dominguez, CA 90220
Phn 310/608-4422
Service Department
Phn 800/367-3165

u Fax [phone]
u Fax [phone]

i

TRAK Bed Mill and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual

Table of Contents

1.0 Introduction

1.1 Manual Organization 1

2.0 Safety 2

2.1 Safety Publication s

2.2 Danger, Warning, Caution and Note
Labels and Notices Used in this Manual

2.3 Safety Precautions

3.0 Description 7

3.1 Control Specifications

3.1.1 Basic System Specifications

3.1.2 Advanced Features Option

3.1.3 Network Option

3.1.4 Installing and using the USB Thumb

Drive Flash Memory

3.1.5 DXF File Converter Option

3.1.6 Converter Options

3.1.7 TRAKing/Electronic Handwheel

Option

3.1.8 How To Buy Software Options

3.2 Display Pendant

3.2.1 Front

3.2.2 Pendant Left Side

3.2.3 Pendant Right Side

3.3 Machine Specifications

3.3.1 SX2, SX3, SX5 Specs

3.3.2 FHM5, FHM7 Specs

3.4 Optional Equipment

3.4.1 Electronic Handwheels

3.4.2 Electronic Head

3.4.3 Position Encoders

3.4.4 Auxiliary Functions

3.4.5 Power Draw Bar

3.4.6 Remote Stop Go Switch

3.4.7 Work Light

3.4.8 Coolant Pump

3.4.9 Spray Coolant

3.4.10 Limit Switches

3.4.11 Chip Pan/Splash Shield

3.4.12 Table Guard

3.5 Lubrication System

3.6 Electrical Cabinet

3.7 Integrated Ram and Quill Encoder

3.9 Servo Motors

4.0 Basic Operation 25

4.1 Switching on the ProtoTRAK SMX CNC

4.2 Shutting down the ProtoTRAK SMX

4.3 Spindle Forward/Off/Reverse

4.4 Manual Operation of Ram, Table, Saddle

4.5 Emergency Stop

4.6 Switching Between Two and Three-Axis
Operation

4.7 Coolant Pump/Spray C ool a nt

4.8 Help Functions

4.8.1 Math Helps

4.9 Windows Up or Down
10 Turning Options On and Off

4.

5.0 Definitions, Terms & Co n cep ts 31

5.1 ProtoTRAK SMX CNC Axis Conventions

5.2 Part Geometry & Tool Path Programming

5.3 Planes and Vertical Planes

5.4 Absolute & Incremental Reference

5.5 Referenced & Non-Referenced Data

5.6 Incremental Reference Position in

Programming

5.7 Tool Diameter Compensation

5.8 Tool Diameter Compensation When

Contouring in Z with Part Geometry

5.9 Connective Events

5.10 Conrad

5.11 Memory & Storage

6.0 DRO Mode 38

6.1 Enter DRO Mode

6.2 DRO Functions

6.3 Jog

6.4 Power Feed

6.5 Do One

6.6 Go to

6.7 Teach

6.7.1 Entering Teach Data

6.8 Return to Absolute Zero

6.9 Spindle Operation

6.10 Tool #

7

.0 Program Mode 43

Part 1: Getting Started & Some General Info

7.1 Programming Overview

7.2 Enter Program Mode

7.3 Program Header Screen

7.3.1 Program Name

7.3.2 General Program Options

7.3.3 Program Header Softkeys

7.4 Auxiliary (AUX) Functions

7.5 Multiple Fixtures

7.5.1 The Default Fixture

7.5.2 Fixtures & Running the Program

7.5.3 Editing Fixtures

7.6 Assumed Inputs

7.7 Z Rapid Positioning

7.8 Softkeys within Events

7.9 Programming Events

7.10 Editing Data While Programming

7.11 LOOK

7.12 Finish Cuts

7.13 Two Versus Three-Axis Programming

ii

TRAK Bed Mill and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual

8.0 Program Mode 54

Part 2: Program Events

8.1 POSN: Position Events

8.2 DRILL Events

8.3 BOLT HOLE Events

8.4 MILL Events

8.5 ARC Events

8.6 POCKET Event

8.6.1 Circular Pocket

8.6.2 Rec tan gu lar Po cket

8.6.3 Irregular Pocket

8.6.4 Tool Path in Pocket Events

8.6.5 Zigzag Z Depth Cuts

8.6.6 Conrad in Pocket Events

8.6.7 Bottom Finish Cut

8.6.8 Face Mill

8.7 Islands

8.7.1 Circular Island

8.7.2 Rectangular Island

8.7.3 Irregular Island

8.8 PROFILE Events

8.8.1 Circle Profile

8.8.2 Rec tan gu lar Pr o f ile

8.8.3 Irregular Profile

8.9 HELIX Events

8.10 SUBROUTINE Events

8.10.1 Repeat

8.10.2 Mirror

8.10.3 Rotate

8.11 COPY Events

8.11.1 Copy Drill to Tap

8.12 THREAD MILL Event

8.13 PAUSE Events

8.14 Tap Events

8.14.1 DPMSX Tapping Speed
Recommendations

8.14.2 FHM5 & FHM7 Tapping Speed

Recommendations

8.14.3 Tapping Notes & Recommendations

8.15 ENGRAVE Event

8.16 Finishing Teach Events

9.0 Program Mode 78

Part 3: The Auto Geometry Engine
(A.G.E) Programming

9.1 Starting the A.G.E.

9.2 A.G.E. Mill Prompts

9.3 A.G.E. Arc Prompts

9.4 Skipping Over Prompts

9.5 The OK/NOT OK Flag

9.6

9.7 Guessing Data

9.8 LOOK and Guess

9.9 Calculated Data

9.10 Arcs and Conrads

9.11 Tangency

Ending A.G.E.

10.0 Edit Mode 85

10.1 Delete Events

10.2 Spreadsheet EditingTM

10.2.1 Selecting Data to be Displayed on
the Search Edit Table

10.2.2 Sorting Data

10.2.3 Making Global Changes to Data

10.3 Erase Program

10.4 Clipboard

10.5 G-Code Editor

11.0 Set Up Mode 92

11.1 The Tool Table

11.1.1 The Tool Table Screen

11.1.2 The Logic of the Tool Table

11.1.3 Initial Tool Set-Up

11.1.4 Starting Over: Erasing Tool Info

11.1.5 Adding a Tool

11.1.6 Replacing a Tool

11.1.7 Z Modifiers

11.1.8 Resetting the Reference Point

11.1.9 Saving Tool Informat i on

11.1.10 Opening a Program

11.1.11 Making Tool Set-Ups Easy

11.1.12 Tool Table & 2-Axis CNC Operation

11.2 Tool Path

11.2.1 Soft Keys in Tool Path

11.3 Reference Positions (REF POSN)

11.3.1 Z Retract

11.3.2 Home Positions

11.3.3 Limit Positions

11.4 Fixture Offsets

11.5 Verify Part

11.6 Service Codes

12.0 Run Mode 104

12.1 Run Mode Screen

12.2 Two Versus Three-Axis Running

12.3 Starting to Run

12.4 Program Run

12.5 TRAKing/Electronic Handwheel Option

12.5.1 TRAKing in Two Axis CNC

12.6 Program Run Messages

12.7 Stop

12.8 Feedrate Override

12.9 Trial Run

12.10 Data Errors

12.11 Fault Messages

12.12 Run Sequence

13.0 Program In/Out Mode 110

13.1 Softkey Selections in the Program
In/Out Mode

13.2 Basic Navigation of Program In/Out Mode
Screens

13.2.1 Basic Parts of the Program In/

Out Mode Screens

13.2.2 Softkeys in the Program In/Out

Mode Screens

13.3 Opening a File

13.3.1 Preview Graphics

13.4 Saving Program Files

13.5 Copying Program Files

iii

TRAK Bed Mill and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual

13.6 Deleting Program Files

13.7 Renaming

13.8 Backing Up

13.9 Converters

13.9.1 Activating Converters

13.9.2 Converting from a Different Format

13.9.3 Converting from the ProtoTRAK CNC

13.10 ProtoTRAK and TRAK CNC Compatability

13.10.1 File Formats

13.10.2 Opening .MX2 & .MX3 Files

13.10.3 Running ProtoTRAK SMX Files on

13.11 Running G Code Files

13.11.1 G Codes Recognized by the
ProtoTRAK SMX CNC

13.11.2 M Codes Supported by the
ProtoTRAK SMX CNC

13.11.3 Valid Characters for Word/Address
Sequences

13.12 Networking

13.12.1 Assigning a Name & Selecting a

13.12.2 A Basic Peer-To-Peer Network

13.12.3 General Information for Advanced

13.12.4 Network Tools on ProtoTRAK SMX

13.12.5 Network Description of the

13.13 CAD/CAM & Post Processors

13.13.1 Writing a Post Processor

13.13.2 Convertible G-Codes

13.13.3 Supported Addresses

13.13.4 Format Terms & Definitions

13.13.5 G Codes that Generate Errors

13.13.6 Accepted M Codes

TM

Into a ProtoTRAK SMX CNC
to a Different Format

ProtoTRAK & TRAK CNC

Workgroup

Networks

ProtoTRAK SMX

1

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CN C Safety, P rogramming, Operating & Care Manual

1.0 Introduction

Congratulations! Your TRAK Bed Mill with the ProtoTRAK SMX CNC is an excellent toolroom
machine. It features an easy-to-use interface and dozens of features that maximize machinist’s
productivity for any kind of toolroom job.

Manual machining is always available and made easier with features like power feed, rapid
positioning, tool offsets and all the best features of sophisticated DRO’s.

Two-axis machining is available at the touch of a button for prototyping and moderately
complex, low volume work.

Three-axis machining is programmed and run with unprecedented flexibility. Programs may
be entered at the control or imported from CAD/CAM files. Advanced color graphics show
program features.

The ProtoTRAK SMX CNC allows you to chose the CNC configuration that is right for you. The
base system is a powerful CNC for toolroom work. You may add opt i ons for additional features
and capabilities.

This manual will describe the operation of all basic and optional features in the appropriate
context. Where optional features are discussed, a note will explain in which option the particular
feature is found.

1.1 Manual Organization

Section 2 of this manual provides important safety information. It is highly

recommended that all operators of this product review this safety information.
Section 3 provides a description of the TRAK Bed Mill and the ProtoTRAK SMX CNC.

Machine Control Options are described in this section.
Section 4 describes the operation of the milling machine and some basic operations of

the ProtoTRAK SMX CNC.
Section 5 defines some terms and concepts useful in learning to program and operate

the ProtoTRAK SMX CNC.
The ProtoTRAK SMX CNC is organized into six Modes of operation that are described in

the following sections.

Section 6 DRO: Digital Readout, jog, and powerfeed operations.
Section 7 Programming, Part 1: covers some general programming information and

instructions on starting new programs.
Section 8 Programming, Part 2: Program Events - instructions for the canned cycles, or

events, used to program the ProtoTRAK SMX CNC.
Section 9 Programming, Part 3: the A.G.E., or Auto Geometry Engine, so powerful it

gets its own section.
Section 10 Edit: for routines to make large-scale changes to programs in current

memory, including the powerful Spreadsheet Editing®

Section 11 Set-Up: Tool information, part graphics and special codes.
Section 12 Run: Instructions on running a program to machine your part.
Section 13 Program In/Out: Storing and managing your programs.

.

2

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CN C Safety, P rogramming, Operating & Care Manual

2.0 Safety

The safe operation of the TRAK Bed Mill depends on its proper use and the precautions taken by
each operator.

• Read and study this manual. Be certain every operator understa nds the operation

before

and safety requirements of this machine

• Always wear safety glasses and safety shoes.

• Always stop the spindle and check to ensure the CNC control is in the stop mode

before changing or adjusting the tool or workpiece.

• Never wear gloves, rings, watches, long sleeves, neckties, jewelry, or other loose
items when operat ing or around the machine.

• Use adequate point of operation safeguarding. It is the responsibility of the
employer to provide and ensure point of operation safeguarding per OSHA 1910.212 ­Milling Machine.

2.1 Safety Publications

its use.

Refer to and study the following publications for assistance in enhancing the safe use of
this machine.

Safety Requirements For The Construction, Care And Use of Drilling, Milling,
and Boring Machines (ANSI B11.8-2001). 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.

2.2 Danger, Warning, Caution, and Note Labels and Notices As Use d
In This Manual

DANGER - Immediate hazards that will result in severe personal injury or death.

Danger labels on the machine are red in color.

could

WARNING - Hazards or unsafe practices that
and/or damage to the equipment. Warning labels on the machine are orange in color.

CAUTION - Hazards or unsafe practices that
equipment/product damage. Caution labels on the machine are yellow in color.

NOTE - Call attention to specific issues requiring special attention or understanding.

result in severe personal injury

could

result in minor personal injury or

3

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual

Safety & Information Labels Used On The

TRAK Bed Mill

It is forbidden by OSHA regulations and by law to deface, destroy or remove any

of these labels

4

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CN C Safety, P rogramming, Operating & Care Manual

220/440 VOLTS

Safety & Information Labels Used On The

TRAK Bed Mill

It is forbidden by OSHA regulations and by law to deface, destroy or remove any

of these labels

5

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual

2.3 Safety Precautions

1. Do not operate this machine before the TRAK Bed Mill Safety, Installation,

Maintenance, Service and Parts List Manual, and t he TRAK Bed Mill Safety,
Programming, Operating & Care Manual have been studied and underst ood.

2. Do not run this machine without knowing the function of e very control key,

button, knob, or handle. Ask your supervisor or a qualified instruct or for help
when needed.

3. Protect your eyes. Wear approved sa fety glasses (with side shields) at all times.

4. Don't get caught in moving parts. Before operating this machine remove all

jewelry including watches and rings, neckties, and any loose-fitting clothing.

5. Keep your hair away from moving parts. Wear adequate safety headgear.

6. Protect your feet. Wear safety shoes with oil-resistant, anti-skid soles, and steel

toes.

7. Take off gloves before you start the machine. Gloves are easily caught in moving

parts.

8. Remove all tools (wrenches, check keys, etc.) from the machine before you start.

Loose items can become dangerous flying projectiles.

9. Never operate a m illing machine after consuming alcoholic beverages, or taking

strong medication, or while using non-prescription drugs.

10. Protect your hands. Stop the ma chine spindle and ensure that the CNC control is

in the stop mode:

• Before changing tool s

• Before changing parts

• Before you clear away the chips, oil or coolant. Always use a chip

scraper or brush

• Before you make an adjustment to the part, fixture, coolant nozzle or
take measurements

• Before you open safeguards (protective shields, etc.). Never reach for
the part, tool, or fixture around a safeguard.

11. Protect your eyes and the machine as well. Don't use a compressed air hose to

remove the chips or clean the machine (oil, coolant, etc.).

12. Stop and disconnect the machine before you change belts, pulley, g ears.

13. Keep work area well lighted. Ask for additional light if needed.

14. Do not lean on the machine while it is running.

15. Prevent slippage. Keep the work area dry and clean. Remove the chips, oil,

coolant and obstacles of any kind around the machine.

6

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CN C Safety, P rogramming, Operating & Care Manual

16. Avoid getting pinched in places where the table, saddle or spindle head create

"pinch points" while in motion.

17. Securely clamp and properly locate the workpiece in the vise, on the table, or in

the fixture. Use stop blocks to prevent objects from flying loose. Use proper
holding clamping atta chments and position them clear of the tool path.

18. Use correct cutting parameters (speed, feed, depth, and width of cut) in order to

prevent tool breakage.

19. Use proper cutting tools for the job. Pay attention to the rotation of the spindle:

Left hand tool for counterclockwise rotation of spindle, and right hand tool for
clockwise rotation of spindle.

20. Prevent damage to the workpiece or the cutting tool. Never start the machine

(including the rotation of the spindle) if the tool is in contact with the part.

21. Check the direction (+ or -) of movement of the table when using the jog or

power feed.

22. Don't use dull or damaged cut ting tools. They break easily and become airborne.

Inspect the sharpness of the edges, and the integr ity of cutting tools and their
holders. Use proper length for the tool.

23. Large overhang on cutting tools w hen not required result in accidents and

damaged parts.

24. Prevent fires. When machining certain materials (magnesium, etc.) the chips

and dust are highly flammable. Obtain special instruction from your supervisor
before machining these materials.

25. Prevent fires. Keep flammable materials and fluids away from the machine and

hot, flying chips.

26. When working in manual mode (not CNC) make sure the computer control is

switched to DRO or OFF.

27. An optional interlocked table guard is available from Southwestern Industries if

the use of the table guard is deemed necessary by the user for his application.

7

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CN C Safety, P rogramming, Operating & Care Manual

3.0 Description

3.1 Control specification s

In its base form, the ProtoTRAK SMX CNC is powerful and easy to use.
The list below summarizes the features and specifications. Each feature is described in more

detail in the appropriate section of the manual.

3.1.1 Basic system s pecifications

Control Hardware

• 2 or 3-axis CNC, 3-axis DRO

• Real handwheels for manual operation

• 10.4” color active-matrix screen

• Industrial-grade Intel® processor

• 256 Mb Ram

• P/S 2 Keyboard connector

• 2 USB connectors

• Override of program feedrate

• LED status lights built into display

• TEAC floppy drive

Software Features – general operation

• Clear, uncluttered screen display

• Prompted data inputs

• English language – no codes

• Soft keys - change within context

• Windows® operating system

• Selectable two or three-axis CNC

• Color graphics with adjustable views

• Inch/mm selectable

• Convenient modes of operation

DRO Mode features for manual machining

• Incremental and absolute dimensions

• Jog at rapid with override

• Powerfeed X, Y or Z

• Do One CNC canned cycle

• Teach-in of manual mo ves

• Servo return to 0 absolute

• Tool offsets from library

Program Mode features

• Geometry-based programming

• Incremental and absolute dimensions

• Automatic diameter cutter comp

• Circular interpolation

• Linear interpolation

• Look –graphics with a single button push

• List step – graphics with programmed events displayed

• Alphanumeric program names

• Program data editing

8

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CN C Safety, P rogramming, Operating & Care Manual

Canned cycles

• Position

• Drill

• Bolt Hole

• Mill

• Arc

• Circle pocket

• Rectangular pocket

• Circular profile

• Rectangular profile

• Program pause

• Conrad – automatic corner radius

• Math helps with graphical interface

• Auto load of math solutions

• Tool step over adjustable for pocket routines

• Pocket bottom finish pass

• Selectable ramp or plunge cutter entry

• Subroutine repeat of programmed events

• Nesting

• Rotate about Z axis for skewing data

Edit mode Features

• Delete events

• Erase program

Set Up Mode Features

• Program diagnostics

• Advanced tool library

• Tool names

• Tool length offset with modifiers

• Advanced diagnostic routines

• Software travel limits

• Tool path graphics with adjustable views

Run Mode Features

• Trial run at rapid

• 3D CAM file program run

• 3D G code file run with tool comp

• Real time run graphics with tool icon

Program In/Out Mode Features

• Simple program storage to floppy

• CAM program converter

• Converter for prior-generation ProtoTRAK programs

3.1.2 Advanced Features Option

The Advanced Features Option may be purchased with the original order or purchased
later. Note, the Advanced Features Option is included in the ProtoTRAK Offline Software,
but must be purchased separately for the ProtoTRAK SMX CNC on the DPM Bed Mill.

It is easy to tell if you have the Advanced Features O ption. If you have the Advanced
Features Option, the features listed below will be active. If you do not, the features
listed below will not be active and any Softkey for that feature will be grayed out. For
example, in the Program Mode under Pocket, check the Softkey labeled IRREG PCKT. If
the words “IRREG PCKT” are black, the Advanced Feature Option is active. If they are
gray, the Advanced Feature Option is not active.

9

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CN C Safety, P rogramming, Operating & Care Manual

The other way to tell if the Advanced Features Option is active is to go to Service Code

318. The Advanced Features Option is active if the letters are in black, inactive if they
are in gray.

With the Advanced Features Option, you get the following:
Auto Geometry Engine ™ (see Section 9.0)

• 3-axis conversational programming

• Additional Canned Cycles:

o Irregular Pocket (8.6.3)
o Face Mill (8.6.8)
o Circle Island (8.7.1)
o Rectangular Island (8.7.2)
o Irregular Island (8.7.3)
o Irregular Profile (8.8.3)
o Helix (8.9)
o Thread milling (8.12)
o Tapping (8.14)
o Engrave (8.15)

• G-Code editor

• Countdown clock to next pause or tool change

• Total program time estimator

• Spreadsheet editing

• Global data change

• Scaling of print data

• Multiple fixture offsets

• Event comments

• Tool path conversational programming

• Mirror of programmed events

• Copy with or without offsets

• Copy Rotate

• Copy Mirror

• Copy Drill to Tap

• Clipboard to copy events between programs

If the Advanced Features Option is not active you may purchase it easily. The Advanced
Features Option is a software option so it is simply a matter of entering the Activation
Password into the ProtoTRAK.

To obtain the Password, see the instructions in section 3.1.8 below.

3.1.3 Networking Option

The Networking Option gives you powerful choices in program storage and handling.
This option may be ordered with your machine or at any time after it is installed in your
shop. A RJ45 port is found on each pendant to hook up your networking cable. See
figure 3.2.2 below for the location of this port.

10

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CN C Safety, P rogramming, Operating & Care Manual

3.1.4 Installing and using the USB Thumb Drive Flash Memory

The first time you install the USB Thumb Drive, we recommend that you install it after
the ProtoTRAK SMX has booted up. Once it is installed, the memory will be accessible on
Drive D. If you want to buy additional thumb drives, these are readily available in
computer stores. We recommend SanDisk® brand, 128MB or higher. Other brands may
require the installation of separate drivers.

3.1.5 The DXF File Converter Option

The DXF File Converter Option gives you powerful capability for quickly and easily
translating DXF and DWG files into ProtoTRAK SMX programs. If you work with CAD
drawings, we highly recommend that you get a demo of the DXF file converter.

• Import and convert CAD data into ProtoTRAK programs

• DXF or DWG files

• Chaining

• Automatic Gap Closing

• Layer control

• Easy, prompted process you can do right at the machine

To tell if the DXF File Converter is active on your ProtoTRAK SMX CNC, go to the options
screen using Service Code #318. If the AutoCAD DXF option is in black letters, it is
activated. If it is in gray letters, you will need to purchase the option to activate it.

The DXF Option Consists of additional software and an Activation Password. The
software can be shipped to you. See Section 3.1.8 below for instructions on ordering and
obtaining your Activation Password.

The DXF Option has its own manual which is shipped with the software. You may also
view a copy of the manual on our web site at www.southwesternindustries.com

.

3.1.6 Converter Options

Optional converters are available for running programs created on other CNCs on the
ProtoTRAK and vice versa.

See section 13.9 for instructions on using converters.
If the converter you want is not active you ma y purchase it easily. C onverters are
software options so it is simply a matter of entering the correct Activation Password into
the ProtoTRAK.

To obtain the Password, see the instructions in section 3.1.8 below.

3.1.7 TRAKing/Electronic Handwheels Option

(Standard on FHM5 and FHM7)

The TRAKing/Electronic Handwheels Option extends the power of the ProtoTRAK SMX
CNC beyond the ordinary by comb ining the electronic handwheels with software routines
in the DRO and RUN Modes. If you did not buy this option with the original machine, you
may add it later.

The option includes:

• Electronic Handwheels on X and Y (replaces the mechanical handwheels, see Section

3.4.1).

• TRAKing of programs during program run (see Section 12.5)

• Go To Dimensions (see Section 6.6)

• Selectable Fine/Coarse handwheel resolution (see Section 3.4.1)

11

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CN C Safety, P rogramming, Operating & Care Manual

Note: If you order this option, do not activate the software for the TRAKing/Electronic
Handwheels Option until the electronic handwheels are installed on the machine. Contact
your local Southwestern Industries, Inc. Sales Representative or the Southwestern
Industries, Inc. Service Department to make arr angements for an authorized technician
to install the electronic handwheels.

3.1.8 How to buy software options.

If you did not buy the software options described above with your machine, you may
purchase them later. In order to use these options, a Software Activation Password is
required. These passwords are unique to your ProtoTRAK SMX CNC.

Software Options are not free. You may call your local Southwestern Industries Sales
Representative or Southwestern Industries Inside Sales at 310-608-4422 for a price
quotation.

1. We recommend that you install the latest version of the ProtoTRAK SMX master
software before installing the newest option. See our web site at
www.southwesternindustries.com for software downloads.

2. Go to the ProtoTRAK SMX CNC on which the opti on is to be installed, use Service
Code 318 to go to the Software Options Scree n.

3. Highlight the option you wish to install (for example, “A: Advanced Features”)
and press the softkey labeled INSTALL.

4. A screen will appear that advises you how to purchase the o ption. Near the
bottom of the screen there will be a Hardware Key Serial Number and an Option
Serial Number. Write down both of these numbers.

5. Call your Southwestern Industries Sales Representative or the Southwestern
Industries Order Desk with your purchase order number and the numbers you
wrote down in step 4 above.

6. When you receive your Password Activation Number, input it into the ProtoTRAK
where indicated on the screen obtained in step 2 above. Some options require
you to reboot the ProtoTRAK to activate.

7. Refer to the appropriate section of this manual for instructions on using your new
features.

12

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CN C Safety, P rogramming, Operating & Care Manual

3.2 Display Pendant

3.2.1 Front

Figure 3.2.1 The ProtoTRAK SMX CNC front panel

Keyboard Hard Keys

Feed Keys:
GO: initiates motion in Run. The green LED on the GO key will be lit when the

servomotors are moving the machine either in jog or when the program run has been
initiated by the GO key.

STOP: halts motion during Run. The red LED on t he STOP key will be lit when the
servos motors are not moving the machine.

13

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CN C Safety, P rogramming, Operating & Care Manual

Override Keys:
F/S: selects the function for th e override operation. F is for feedrate. When the LED

above the F is lit, arrow presses will increase or decrease axis feedrate. S is for
spindle RPM. When the LED above the S is lit, arrow presses will increase or
decrease the spindle RPM. Note: the spindle override is active only when the
Programmable Electronic Head is installed.

é: Feedrate Override to increase feedrate or spindle rpm up to 150%.
ê: Feedrate Override to decrease feedrate or spindle rpm down to 10%.

Each button push Modifies the feedrate in 10% increments and the spindle speed in
5% increments.

ACCESSORY: When the switch is in the On position, the flood coolant pump (or
spray coolant) will come on and stay on during machining operations. In the Auto
mode, the coolant pump or spray coolant will be controlled as programmed by the
Auxiliary functions. To get to the Auto operation, press and hold the Accessory key.
If neither light is on, the coolant pump or spray coolant will not operate.

F/C: Selects between fine and course resolution for the X and Y handwheels when
the TRAKing/Electronic Handwheels Option is installed. The LED above the letter
indicates which feed is active. Fine feed moves the axis .200 inches per revolution.
Course feed moves .800 inches per revolution.

INC SET: loads incremental dimensions and general data
ABS SET: loads absolute dimensions and general data
INC/ABS: switches all or one axis from incremental to absolute or absolute to incremental
IN/MM: causes Inch to Metric or Metric to Inch conversion of displayed data
LOOK: part graphics in Program mode
X, Y, Z: selects axis for subsequent commands

RESTORE: clears an entry, aborts a keying procedure

0-9, +/-, . : inputs numeric data with floating point format. Data is automatically + unless
+/- key is pressed. All input data is automatically rounded to the system's resolution.

MODE: to change from one mode of operation to another

SYS:

3-axis to 2-axis operation, and other functions.

To shut down the ProtoTRAK SMX C NC, change from 2-axis to 3-axis, or

p : reinstates a window.
q : eliminates a window.

HELP: displays help information, math help or additional functions. Active for
additional functions when the help symbol (a blue question mark) is displayed on the
screen next to the HELP key.

14

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CN C Safety, P rogramming, Operating & Care Manual

Soft Keys:

Beneath the display are 8 keys that are labeled with arrows. These keys are called software
programmable or soft keys. A description of the function or use of each of these keys will be
shown at the bottom of the display directly above each key. If, at any time, there is no
description above a key, that key will not operate.

Sometimes the description or function of the key is visible but grayed out. This indicates
that the particular function is not available because of some other condition. For
example, if the Z retract is not set, the RUN mode key will be grayed out because setting
the Z retract is a necessary step for running a program.

Emergency Stop Switch

The emergency stop (E-stop) switch kills all power to the spindle and ProtoTRAK's servomotors.
The computer and pendant remain powered.

The Liquid Crystal Display (LCD)

The display of the ProtoTRAK SMX CNC is a 10.4" active-matrix color LCD. The very top is the
Status Line that shows the overall status of the ProtoTRAK SMX CNC. This includes the current
Mode, the current program part number, the current tool number, 2 or 3-axis mode and
whether the X, Y and Z dimensions are in inch or millimeter (mm).

Just above the soft keys is a data input line that appears when an input is required

.

15

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CN C Safety, P rogramming, Operating & Care Manual

3.2.2 The ProtoTRAK SMX CNC left side with connectors labeled

3.2.2 Pendant Left Side (See Figure 3.2.2)

FIGURE

16

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CN C Safety, P rogramming, Operating & Care Manual

3.2.3 The ProtoTRAK SMX CNC right side

3.2.3 Pendant Right Side (See Figure 3.2.3)

FIGURE

17

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CN C Safety, P rogramming, Operating & Care Manual

Pendant Right Side with USB Ports

Keyboard P/S2 port. This port is for the keyboard only. If this port is used, the connection

must be made before the ProtoTRAK is turned on. If the ProtoTRAK is already on, it will not
recognize the keyboard until it is rebooted with the keyboard plugged in. You may also plug the
keyboard into one of the USB ports.

USB Ports. The USB ports are the only ports available for plugging in a mouse. They may also
be used for a keyboard or for plugging in USB Thumb Drive flash memory. Items used by USB
ports will be recognized even if they are plugged in after the ProtoTRAK is turned on.

If you need more than the available number of USB ports, we recommend that you install a USB
hub. If you use the USB Thumb Drive to store a G-code (.gcd) program file, you must leave the
Thumb Drive plugged into the USB port the entire time the program is in current memory. If you
unplug the thumb drive with the program still in current memory, the ProtoTRAK will display an
error message.

Drivers for most major brands of mouse and keyboard are already in the ProtoTRAK SMX. If a
mouse or keyboard is not recognized by the ProtoTRAK, it means that the driver is not available.
Loading a new driver is not difficult for a qualified computer administrator who can access the
start menu on the ProtoTRAK with a keyboard plugged in (see the Catch 22?). However, most
users would be happier to simply go get a keyboard and mouse that are already supported. We
recommend Microsoft, Logitech and Belkin brand products.

AC on/off. The ProtoTRAK should be shut down properly before turning off (Sections 4.1 and

4.2).

18

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CN C Safety, P rogramming, Operating & Care Manual

FIGURE 3.3.1 The TRAK DPM SMX Series machine overview

3.3 Machine Specifications

(See Figures 3.3.1 and 3.3.2)

3.3.1 DPMSX2, SX3 and SX5 Specifications

19

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CN C Safety, P rogramming, Operating & Care Manual

3.3.2

FIGURE

The TRAK DPMSX3 Series back view

20

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CN C Safety, P rogramming, Operating & Care Manual

MODEL NAME

DPM SX2

DPM SX3

DPM SX5

Spindle Speed Range with E Head

40-600, 300-5000

Spindle Motor Power – vari-speed head

3 HP

5 HP

Power requirements, control

110V; 1P; 8A

Power requirements, machine with

220V;3P; 11A

220V;3P; 17A

Height of table from bottom of bed

33”

38”

41”

Min height

90”

85"

87”

Width of machine including tab le

70”

73”

94”

Overall width incl full table traverse

104”

108”

136”

Footprint of Machine

23 x 40”

24” x 44”

24” x 48.4”

Drilling max capacity – Varispeed head

3

Tapping max capacity – Varispeed head

3

Table Size 49x9 50” x 10” 50” x 12”
T-Slots (number x width x pitch) 3 x .63” x 2.5” 3 x .63" x 2. 48" 3 x .63" x 2.52"
Travel (X, Y, Z axis) 32 x 16 x 27 30 x 17 x 23.5" 40 x 20 x 23.5”
Quill Diameter 3 3/8” 3 15/16"
Maximum Quill Travel 5”
Spindle Taper R8 NST 40
Spindle Speed Range RPM – Varispeed
drive

Option (standard feature as of 1/1/11)
Spindle Center to Column Face 18” 19” 20”

Spindle Motor Power – Optional E head
(standard feature as of 1/1/11)

Power requirements, machine with
vari-speed head

Optional E head
Maximum Weight of Workpiece 1320 lbs. 1760 lbs.

Max spindle nose to table 27” 23.5”

70-4200 70-3950

3 HP 5 HP

220/440;3P;

8.5/4.25A

220/440V;3P; 14/7A

Max height 98” 95” 98”

Length with electric box door closed 64” 60” 67”

Overall length with electrical door open 72” 70" 77"

Weight net / shipping lbs. 3200 / 3500 4100 / 4400 4400/ 4600
rapid traverse X, Y, Z

150 IPM 150 IPM

Maximum Work Capacit i es in M il d Steel

1” dia

Milling max capacity – Varispeed head

Drilling max capacity – Optional E head
Milling max capacity – Optional E head
Tapping max capacity – Optional E head

2 inch

3 inch

/min 5 inch3/min 5 inch3/min

5/8” 1" 1”

1”

/min 5 inch3/min

3 /4 - 10 1 - 8

21

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CN C Safety, P rogramming, Operating & Care Manual

MODEL NAME

FHM5

FHM7

T-Slots (number x width x pitch)

3 x 16mm x 63.5mm

4 x 16mm x 63.5 mm

Quill Diameter

4.13”

5.06”

Spindle Speed Range RPM

160 – 4000

200 – 5000

Spindle Motor Power

5 HP

7.5 HP

Power requirements, machine

220V / 3P / 60HZ

220V / 3P / 60HZ

Maximum Weight of Workpiece

1760 lbs.

2200 lbs.

Max spindle nose to table

24”

24”

Drilling Max Capacity

1” dia.

1” dia.

Tapping Max Capacity

5/8”

5/8”

3.3.2 FHM5 and FHM7 Specifications.

Table Size 50” x 12” 78” x 14”

Travel (X, Y, Z axis) 40” x 20” x 24” 60” x 23” x 20.5”

Spindle Taper NMTB 40 NMTB 40

Spindle Center to Column Face 20.5” 23”

Power requirements, control 110V / 1P / 15A 110V / 1P / 15A

Current (Full load Amp) 17.5 FLA 37.5 FLA

Height of table from bottom of bed 41” 38.25”

Min height 87” 95.5”
Max height 100” 101”
Width of machine including tab le 94” 110.5”
Length with electric box door closed 80” 93.75”
Overall width incl full table traverse 136” 171.65”
Overall length with electrical door open 105” 119.5”
Footprint of Machine 24” x 48.4” 42.52” x 63”
Weight net / shipping lbs. 4400 / 4700 7650 x 7975
rapid traverse X, Y, Z 250 IPM 250 IPM

Maximum Work Capacities in Mild Steel

Milling Max Capacity 5 inch3 / min 7 inch3 / min

3.4 Optional Equipment

3.4.1 Elec tronic Handwheels

Models FHM5 and FHM7 have electronic handwheels as standard.
When ordered as part of the TRAKing/Electronic Handwheels Option (see Section 3.1.7)

the electronic handwheels replace the standard mechanical handwheels for table and
saddle traverse. The electronic handwheels will operate when the ProtoTRAK SMX CNC is
in a Mode where the machinist controls the motion of the table and saddle. This includes
the DRO Mode, the Set-Up Mode and the TRAKing operation in the Run Mode. The
electronic handwheels will not operate during other functions, such as when the “Select a
Mode” message appears on the screen.

Handwheel resolution is determined by the F/C key on the display. Fine feed moves
.200 inches per revolution, Course feed moves .800 inches per revolution.

22

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CN C Safety, P rogramming, Operating & Care Manual

3.4.2 Electronic Head

Models FHM5 and FHM7 have the electronic head as standard. The electronic head
became a standard feature as of 1/1/11 on all DPM’s.

When ordered as the Programmable Electronic Head Option, the electronic head replaces
the mechanical head and manual vari-speed control. The electronic head retains manual
quill control, down feed selection knobs and the manual forward/off/reverse switch. The
Tap Event is also activated with this option (Section 8.14).

Spindle speed settings and overrides are performed using the ProtoTRAK SMX CNC. See
Sections 6.9 and 12.8 . In addition, the spindle speed becomes part of the programming
of the canned cycles (Section 8, Program Events).

See the specifications table above for the different electrical requirements for the
electronic head.

This option is available factory-installed only. It is not available after shipment.

3.4.3 Position Encoders

The ProtoTRAK SMX CNC may be configured to run either with or without independent
position encoders for X and Y travel. Optional encoders include the TRAK sensors or
glass scales, each with .0002” underlying resolution. The TRAK sensor option is not
available for the FHM7.

3.4.4 Auxiliary Functions

Auxiliary functions are control led through the ProtoTRAK SMX CNC either in the program
or with the accessory key on the front panel. The Auxiliary functions consi st of the
following:

• Spindle off command

• An air solenoid to control spray coolant or other pneumatically activated peripheral

equipment. Shop air should not exceed 125 psia.

• Switched and fused 120 VAC 8 Amp outlet for coolant pumps, automatic oilers, etc.

• INPUT/OUTPUT to interface with programmable indexers, dividing heads, etc.

o Output from ProtoTRAK SMX CNC is .3-second actuation of a solid-state relay

between pin 3 (plus), a nd pin 4 (minus).

o Input to the ProtoTRAK SMX CNC is .3-second actuation of a solid-state relay

between pin 1 (plus), a nd pin 2 (minus).

o Note: Pin 1 is on top, 2 on right, 3 on left, 4 on bottom.

.

3.4.5 Power Draw Bar

A manual draw bar, o f the NMTB or NST type comes standar d with the machine. A
power draw bar option may be ordered. The draw bar included in the option may be
CAT or NMTB/NST.
An NMTB/NST type of draw bar is the appropriate length to fit tool holders that have a
threaded tang on the top. The CAT type is longer to thread into CNC tool holders that
have the tool changer grip, or retention knob removed.

3.4.6 Remote Stop Go Switch

For the convenience of operation while running the program, a Remote Stop/Go switch
may be purchased. This switch is on a ten-foot cable and operates like the FEED Stop
and Go keys on the display.

23

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CN C Safety, P rogramming, Operating & Care Manual

CAUTION!

3.4.7 Work Light

An optional halogen work light is available. It mounts to the left side (facing) of the
column and plugs into a 110v outlet in the electrical cabinet.

3.4.8 Coolant Pump

The optional coolant pump is mounted in the back of the machine co lumn. It is plugged
into the electrical cabinet and may be configured to operate as commanded by the
auxiliary functions, or with a separate switch.

3.4.9 Spray Coolant

The Fog Buster® spray coolant option consists of a one-gallon holding tank, nozzle, air
lines and an air regulator for attaching compressed air. Coolant flow is adjusted by a
needle valve at the sprayer head. Air flow is adjusted at the air pressure regulator wit h
gage. Once flows are set, sprayer operation is controlled by an air toggle switch or by
interface with the optional Auxiliary Functions.

3.4.10 Limit Switches

There are optional limit switches for the ram, saddle and table travel.

3.4.11 Chip Pan/Splash Shield

The Chip Pan/Splash Shield option consists of a chip pan mounted to the bed and splash
shields mounted to the right and left of the columns. This option is available factory­installed only. It is not available after shipment.

3.4.12 Table Guard

The Table guard option provides an enclosed workspace mounted on the table. The
sliding door is switched to prevent operation of the CNC Run with the door open. While it
will aid in the control of chips and coolant, it is not a full, waterproof enclosure.

3.5 Lubrication System

The way and ballscrew lubrication pump is wired to operate when the spindle is running.
Factory Default Values

Interval Time – 60 min.
Discharge Time – 15 sec
Discharge Pressure – Approximately 100 – 150psi

To adjust the amount of Discharge Pressure displayed on the lube pump gauge, loosen
the jam nut and turn the adjustment screw located o n the top right side of the lube
pump while the lube pump is activated. To activate the lube pump turn spindle on and
press the Feed for continuous pumping and RST for a single progr ammed pump.

CAUTION!

Failure to properly lubricate the mill will result in the premature failure of bearings and sliding surfaces.

Failure to manually activate the pump at the beginning of each day, or allowi ng the Auto Lube to run
dry may cause severe damage to the machine mill way surfaces and ballscrews.

24

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CN C Safety, P rogramming, Operating & Care Manual

The settings for the lube pump can be viewed by doing the following: press Service
Codes, press “A” (software), press Code 313. This screen lists the values programmed
for the cycle time and discharge time.

3.6 Electrical Cabinet

The TRAK Bed Mill uses two electrical inputs. Spindle 220 or 440V power i s wired into
the cabinet. A cord is supplied from the cabinet to a 110V power source for running the
ProtoTRAK SMX CNC. 440V is not available for machines with the Programmable
Electronic Head .

3.7 Integrated Ram and Quill Encoders

A glass scale for the Quill operation is standard. Ram motion is measured by an encoder
on the ram servo motor. The feedback from these encoders is integrated and displayed
in the Z-axis digital readout as one dimension.

3.8 Servo Motors

The servo motors on table, saddle and ram are 560 in-oz torque. Integrated into each
motor is an encoder with 0.000068” underlying resolution.

25

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CN C Safety, P rogramming, Operating & Care Manual

4.1.1 The main “select a mode” screen. Shown here, the Edit and Run Modes are grayed

out because there is no program in current memory

4.0 Basic Operation

One of the things that makes the TRAK DPM so easy to use is that most of the operations of the
ProtoTRAK SMX CNC are organized in Modes. Modes are logical groups of activities that naturally
belong together. This eliminates the need to memorize operations – just select a mode and
choose among the soft keys.

Most operations will be discussed within the section that treats the mode later in this manual.
The operations described in this section either don’t fit in a particular mode, or they are relevant
to more than one mode.

4.1 Switching on the ProtoTRAK SMX CNC

To turn the ProtoTRAK SMX CNC on, move the toggle switch on the display side panel to the Up position.
The Windows operating system and the ProtoTRAK SMX CNC software will take a few seconds to

load from the system's flash memory. If you have connected the ProtoTRAK SMX CNC to a
network, it may take as long as 90 seconds for the communications to be established. When
complete, the ProtoTRAK SMX CNC Select Mode screen will appear.

Select the Mode of operation by pressing the soft key beneath the labeled box. Notice that the
EDIT and RUN soft keys are grayed out when the system is first turned on. They will not function
because there is no program in the ProtoTRAK SMX CNC . Once a program is entered, the EDIT
key will function. Once a program is entered and the necessary SET-UP operations are complete,
the RUN key will function.

FIGURE

The ProtoTRAK SMX CNC has a screen saver already programmed in. If the system is not used
(either by a key stroke or by counting) for 20 continuous minutes, the display will turn itself off.
The LED’s on the keypad will flash every few seconds to indicate that the system is still on. Press
any key or move any axis to bring the screen back to its previous display. The key you press will
be ignored except to turn the screen on.

26

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CN C Safety, P rogramming, Operating & Care Manual

FIGURE 4.6 You will see this screen when the SYS hard key is pressed. The choice

4.2 Shutting down the ProtoT RAK SMX CNC

Important: the system must be turned off properly. First press the SYS hard key and

then press the SHUT DOWN soft key (see Figure 4.6). After a few seconds, you will see
the message "it is now safe to turn off your computer". Turn the ProtoTRAK SMX CNC off
by moving the toggle switch on the display side panel to the down position.

If the CNC is not shut down properly you may lose unsaved data such as programs or
certain machine configurations.

Note: When you turn the PROTOTRAK SMX CNC off, always wait a few seconds before turning it back on.

4.3 Spindle Forward/Off/Reverse

The spindle is controlled thr ough the drum switch mounted on the side of the machine head.

4.4 Manual Operation of the Ram, Table & Saddle

The TRAK DPMSX2, DP MSX3 or DPMSX5 may be used manually (see 3.4.1 for electronic
handwheel operati on). The head/ram may be jogged to any location and the quill
operated manually. Either motion will count in Z.

4.5 Emergency Stop

Press the button to shut off power to the spindle motor and axis motors. Rotate the

switch to release.

4.6 Switching Between Two and Three-axis Operation

The ProtoTRAK SMX CNC may be operated as a two or three-axis CNC. Press the SYS
hard key. Softkey F2 will read GO TO 2 AXIS when the ProtoTRAK SMX CNC is currently
operating in three axis and it will say GO TO 3 AXIS when the ProtoTRAK SMX CNC is
currently operating in two axis. See Figure 4.6.

“GO TO 2 AXIS” shows that the CNC is currently in 3-Axis operation.

27

Southwestern Industries, Inc.

TRAK Bed Mills and ProtoTRAK SMX C NC Safety, P rogramming, Operating & Care Manual

4.8.1 The first Math Helps screen. Choose among the alternatives based on the

4.7 Coolant Pump/Spray Coolant

An optional coolant system may be connected to your DPM. If you do not have the
Auxiliary Functions option, manual control s for the system are provided. If you do have
the optional Auxiliary Functions, the operation of the coolant system may be programmed
within the program events. With the Auxiliary Functions s et-up, manual control of the
coolant system is through the Accessory key on the front panel of the SMX CNC.

To operate the mister or coolant pump manually, use the ACCESSORY hard ke y:

• ON - will turn on the mister or coolant pump until you tur n i t off.

• AUTO - will turn on the mister or co olant pump on, as programmed into events.

• Off (no light) - the coolant pump or mister stays off.

4.8 Help Functions

When a blue question mark appears next to the HELP hard key, that means special
functions or configuration settings are available for the current operation. For example,
at the program header with the highlight on the program name, the blue question mark
appears. Pressing the HELP key at that time will call up a table with alpha and special
characters you can use to name your program.

4.8.1 Math Helps

When the blue question mark does not appear, pressing HELP will initiate the Math
Helps.

FIGURE

information you need to calculate

28

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CN C Safety, P rogramming, Operating & Care Manual

Math Helps are powerful routines that enable you to use the data you have available to
calculate missing print data.

For example, Math Help type 28 enables you to solve an entire right triangle by giving
two known pieces of data. To exit from the Math Help, press the Mod e key.

29

Southwestern Industries, Inc.

TRAK Bed Mills and ProtoTRAK SMX C NC Safety, P rogramming, Operating & Care Manual

FIGURE 4.8.2 Math Help 28. In this example, by entering the length of line A and the value of

angle G, the other values are calculated

You may have the Math Help solutions load directly into your program. This saves you
from having to write down the solution and then key it in. While you are programming
the event that needs the data from Math Help, simply press the HELP key to start the
Math Help. Once a solution is obtained, you will have the following soft key selections:

Load Begin: will load the displayed solution into the event as the X and Z beginning.
Load End: will load the displayed solution into the event as the X and Z end.
Load Center: will load the displayed solution into the event as the X and Z center.
Next Solution: when there is more than one solution to the problem, this will display

the alternative solutions.
Edit: this allows you to go back to the data you entered in order to make changes. Once

you do this, the Resolve key will appear.

Resolve: press this to have the Math Help use the new data to give new solutions.

4.9 Windows Up or Down

Some of the selections in the ProtoTRAK SMX CNC will cause a window to appear with a
message. To eliminate the window in order to see what is behind it, press the u hard
key. To restore the window, press the t hard key.

4.10 Turning Options On and Off

If the Advanced Feature s Option has been installed, you may run the ProtoTRAK SMX
with it turned off. This has the benefit of making the system easier to use.

30

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CN C Safety, P rogramming, Operating & Care Manual

To turn the options on or off, press the SYS hard key. You will get the screen shown in
Figure 4.6 above. Press the Options On/Off softkey. This will take you directly to the
screen that will all ow you to turn options on and off. You can also get to this screen
using Service Code 334.

The Programmable E-Head Option and TRAKing/Electronic Handwheel Option may not be
turned on or off. If they are installed, they must remain active.

31

Southwestern Industries, Inc.

TRAK Bed Mills and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual

5.1 ProtoTRAK SMX CNC conventions

5.0 Definitions, Terms & Concepts

5.1 ProtoTRAK SMX CNC Axis Conventions

X Axis: positive X-axis motion is defined as the table moving to the left when facing the

mill. Consequently, measurement to the right is positive on the workpiece.
Y Axis: positive Y-axis motion is defined as the table moving toward you. Measurement

toward the machine (away from you) is positive on the workpiece.
Z Axis: positive Z-axis motion is defined as moving the head up. Measurement up is

also positive on the workpiece.

FIGURE

The Z RAPID dimension is the position at which Z will stop rapid traversing and switch to
its programmed Z feedrate. Z motion will continue until Z End depth has been reached.

5.2 Part Geometry & Tool Path Programming

The ProtoTRAK SMX CNC gives you ultimate flexibility in programming. Programs that are
entered through the ProtoTRAK SMX CNC system can be entered as either Part Geometry or Tool
Path (optional).

Part Geometry programming is the popular programming style of the ProtoTRAK family of
products. This is done by defining the final geometry of the part, and the ProtoTRAK
SMX CNC has the job of figuring out the tool path from the part dimensions and the tool
set-up information. This is a great benefit compared to regular CNC because it doesn't
force the programmer to do the difficult job of defining tool path. A consequence of part
geometry programming is that the following are not allowed:

• connectio n of an incline plane and another event

• connecti on of two events that lie in different planes

Using Geometry Programming, it is impossible for the ProtoTRAK SMX CNC to calculate a tool
path for these cases without creating a problem: in cutting the geometry desired in the first
event, the tool ends up out of position for the next event. Resolving the difference in tool
position where the first event ends and the next event begins means either the CNC calculates
and makes an unprogrammed move, or it retra cts the tool out and then back into the part.

_________________________________________________________________

32

Southwestern Industries, Inc.

TRAK Bed Mills and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual

FIGURE 5.3 Vertical planes

These cases are not encountered often, but when they are you have the option of using Tool
Path programming. In Tool Path programming you define the events the same way, but all
inputs are treated as tool center. It is your job to calculate and program the tool path.

Note: Tool Path programming is part of the Advanced Features Option.
Programs generated by CAD/CAM systems are always generated as Tool Path programs and are

run as such even if the Advanced Features Option has is not active on the ProtoTRAK SMX CNC.

5.3 Planes and Vertical Planes

A plane is any flat surface. If that surface lies flat on the table, it is the XY plane. That is, if you
move your finger along that surface or plane, you are moving in the X and/or Y direction, but not
in Z (or at least not until you pick your finger up). If you tilted that surface (think of it as a piece
of paper) straight up so that it faces the front of the machine, it would be in the XZ plane. If you
tilted it up so that it faced left or right, it would be in the YZ plane .

A vertical plane is any plane (or surface) tipped up on its edge on the table (see below).
Programming vertical planes requires the Advanced Features Option (Section 3.1.2).

Unlike most CNC controls,
the ProtoTRAK SMX CNC can
machine arcs in any vertical
plane rather than just XZ or YZ.

5.4 Absolute & Incremental Reference

The ProtoTRAK SMX CNC may be programmed and operated in either (or in a combination) of
absolute or incremental dimensions. An absolute reference from which all absolute dimensions
are measured (in DRO and program opera tion) can be set at any point on or even off the
workpiece.

To help understand the difference between absolute and incremental position, consider the
following example:

33

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CN C Safety, P rogramming, Operating & Care Manual

5.4 Each point has both an absolute and an incremental reference in the X axis. The

ProtoTRAK SMX CNC allows you to program using either.

FIGURE

5.5 Referenced & Non-Referenced Data

Data is always loaded into the ProtoTRAK SMX CNC by using the INC SET or ABS SET
key. X, Y, Z positions are referenced data. In entering any X, Y, or Z position data, you
must note whether it is an incremental or absolute dimension and enter it accordingly.
All other information (non -referenced data), such as tool diamete r, feedrate, etc. is not a
position and may, there fore, be loaded with either the INC SET or ABS SET key. This
manual uses the term SET when either INC SET or ABS SET may be used
interchangeably.

5.6 Incremental Reference Position in Programming

When X, Y, Z RAPID and Z data for the beginning position of any event are input as
incremental data, this increment must be measured from some known point in the
previous event. Following are the positions for each event type from which the
incremental moves are made in the subsequent event:

Position: X, Y and Z programmed
Drill: X, Y, Z RAPID, and Z END programmed
Bolt Hole: X CENTER, Y CENTER, Z RAPID and Z END programmed
Mill: X END, Y END, Z RAPID and Z END programmed
Arc: X END, Y END, Z RAPID and Z END programmed
Circle (POCKET or FRAME): X CENTER, Y CENTER, Z RAPID and Z END programmed
Rectangle or Irregular (POCKET or PROFILE): X1 and Y1 corner, Z RAPID and Z

END programmed
Helix: The X END, Y END, Z RAPID, and Z END progra mmed. Helix programming

requires the Advanced Features Option.
Sub: The reference position as defined for the specific events above for the event prior

to the first event that was repeated.
A.G.E. PROFILE: The appropriate reference position as defined for the specific events

above for the last event that is programmed. A.G.E. Profile Programming requires the
Advanced Features Option.

34

Southwestern Industries, Inc.

TRAK Bed Mills and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual

5.7.2

For example, if an ARC event followed a MILL event, a 2.0 inch incremental X BEG would
mean that in the X direction the beginning of the ARC event is 2.0 inches from the end of
the MILL event.

5.7 Tool Diameter Compensation

Tool diameter compensation allows the machined edges shown directly on the print to be
programmed instead of the center of the tool. The ProtoTRAK SMX CNC then
automatically compensates for the programmed geometry so that the desired results are
obtained.

Tool cutter compensation is always specified as the tool either right or left of the
workpiece while looking in the direction of the tool motion.

FIGURE 5.7.1 Examples of tool right

Tool center means no compensation either right or left. That is, the centerline of the tool
will be moved to the programmed points.

FIGURE

Examples of tool left

35

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CN C Safety, P rogramming, Operating & Care Manual

FIGURE 5.8.1 Ball end mill position with respect to program points. Tool starts so end mill is

tangent to BC. R from center of tool is perpendicular to BC

5.8.2 In order to respect the lines defined by the programmed points, the ball end mill

never touches point B. Tool starts centered over A offset up by the tool

radius R. It moves right until it is tangent to both AB and BC. Then moves to

point C as in the first example

5.8 Tool Diameter Compensation when Contouring in Z with Part Geometry

Note: Z contouring requires the Advanced Features Option (Section 3.1.2)
Left and right tool diameter offsets are always those projected into the XY plane. Tool

offsets in the Z direction are always up and assume the use of a ball end mill. When
contouring in the Z-axis, this up tool offset is always activated regardless of left, right,
center if the Part Geometry option is selected. There is no Z-axis up tool offset applied
when the Tool Path option is selected.

Special attention must always be paid to tool offsets when machining with a ball end mill.
The reason for this is that the tool diameter changes in the bottom part (that portion
equal to the tool radius) of the tool.

The tool is always positioned at the beginning o f a milling operation so that the correct
point on the ball end of the tool is tangent to the beginning point, and offset perpen­dicular to the machined edge by the radius of the tool. Consider the example below of
milling a ramp in the XZ plane from point B to point C.

FIGURE

Note how the tool at the beginning point (point B) starts below (in the Z direction) point
B so that it can actually touch this point. If this were not true, a cusp would remain to
the left of point B.

Now consider a similar example milling from A to B to C in the XZ plane.

Note the Tool at B does not drop below the AB line and, therefore, never touches point B.
As a result, a fillet is formed at point B equal to the tool radius.

This second example of continuous m achining from one cut (AB) to another (BC) with full
cutter compensation between requires the two cuts to be made with events which are
connective (see Section 5.9 or 5.10 for a more complete discussion of this requirement).

36

Southwestern Industries, Inc.

TRAK Bed Mills and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual

FIGURE 5.10.1 A Conrad is added between the two intersecting lines

5.9 Connective Events

Connective events occur between two milling events (either Mill or Arc) when the X, Y, and Z
ending points of the first event are in the same location as the X, Y, and Z starting points of the
next event. In addition, the tool offset and tool number of both events must be the same. And
both events must lie in the XY plane or the same vertical plane (see Section 5.2).

5.10 Conrad

Conrad is a unique feature of the PROTOTRAK SMX CNC that allows you to program a
tangentially connecting radius between connective events, or tangentially connecting radii for the
corners of pockets and frames without the necessity of complex calculations.

For the figure below, you program an Arc event from X1, Y1 to X2, Y2 with tool offset left, and
another Arc event from X2, Y2 to X3, Y3 also with tool offset left. During the programming of the
first Arc event, the system will prompt for Conrad at which time you input the numerical value of
the tangentially connecting radius r=K3. The system will calculate the tangent points T1 and T2
and direct the tool cutter to move continuously from X1, Y1 through T1, r=K3, T2 to X3, Y3.

Note: Conrad must always be the same as or larger than the tool radius for inside corners. If Conrad is
less than the tool radius, and an inside corner is machined, the ProtoTRAK SMX CNC will ignore the
Conrad.

37

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CN C Safety, P rogramming, Operating & Care Manual

FIGURE 5.10.2 A Conrad is added between an arc and a line

For the figure below, you program an Arc event from X1, Z1 to X2, Z2, and a Mill to X3, Z3.
During the programming of t he Arc event, the system will prompt for Conrad at which time you
input the numerical value of the tangentially connecting radius r=K. The system will calculate the
tangent points T1 and T2 and direct the tool cutter to move continuously from X1, Z1 through T1,
r=k, T2 and on to X3, Z3.

5.11 Memory & Storage

Computers can hold informa tion in two ways. Information can be in current memory
or in storage. Current memory (also known as RAM) is where the ProtoTRAK SMX CNC
holds the operating system and any part program that is ready to run. While a program
is being written, it is in current memory.

Storage of programs can be done on a USB device or on a disk in the floppy drive. We
strongly recommend yo u habitually back up programs.

When the Network Option is purchased, program storage can also be saved to an offline
computer that is networked to your SMX CNC.

38

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CN C Safety, P rogramming, Operating & Care Manual

FIGURE 6.1 The DRO screen

6.0 DRO MODE

The ProtoTRAK SMX CNC operates in DRO Mode as a sophisticated 3-axis digital readout with jog
and power feed capability.

6.1 Enter DRO Mode

Press MODE, select DRO soft key. The CRT screen will show:

Note the RETURN soft key is lit when in Jog or Power Feed operation.

6.2 DRO Functions

Clear Entry: Press RESTORE, then re-enter all keys.
Inch to MM or MM to Inch: Press IN/MM and note LCD screen status line.
Reset One Axis: Press X or Y or Z, INC SET. This zeros the incremental position in the

selected axis.

Preset: Press X or Y or Z, numeric data, INC SET to preset selected axis.
Reset Absolute Reference: Press X or Y or Z, ABS SET to set selected axis absolute to

zero at the current position.

Note: This will also reset the incremental dimension if the absolute position is being
displayed when it is reset.

39

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CN C Safety, P rogramming, Operating & Care Manual

Preset Absolute Reference: Press X or Y or Z, numeric data, ABS SET to set the
selected axis absolute to a preset location for the current machine position.

Note: This will also reset the incremental dimension if the absolute position is being displayed
when it is preset.

Recall Absolute Position of All Axes: Press INC/ABS. Note the dimension for each axis is
labeled INC or ABS. Press INC/ABS again to revert to the original reading.

Recall Absolute Position of One Axis: Press X or Y or Z, INC/ABS. Note the INC or
ABS label for each axis. Repeat to get selected axis back to original reading.

6.3 Jog

The servomotors can be used to jog the table, saddle and ram.

a. Press the JOG soft key.
b. A flashing message will appear saying "CAUTION: JOG KEYS ARE ACTIVE".
c. To jog, press the X, Y or Z hard keys.
d. To stop jogging, release the key.
e. The speed of jog is displayed in the box next to the words "Feed Rate” on the

lower left side of the LCD screen.
f. Press the +/- hard key to reverse direction. When the number in the Feed rate

box is negative, this indicates the minus direction.

d. Press the RATE keys to reduce and to increase the jog speed in 10
percent increments. The changes in speed may be seen in the Feed rate box
and on the green feed rate indicator. The amount of override is displayed in
the Override box.

g. To jog at a certain rate, simply enter that number as inches or mm per minute and
then press the X, Y or Z key. You may also use the override key to adjust this number.
Press RSTR to return to 150 ip m or 3800mm/min.

h. Press RETURN soft key to return to manual DRO operation.

6.4 Power Feed

The servomotors can be used as a power feed for the table, saddle or quill, or all three

simultaneously.
a. Press the POWER FEED soft key.
b. A me ssage box will appear that shows the power feed dimensions. All power feed

moves are entered as incremental moves from the current position to the next
position.

c. Enter a position by pressing the axis key, the distance to go and the +/- key (if

needed). Input the entry b y pressing INC SET. For example, if you wanted to

make a power feed move of 2.00" of the table in the negative direction, you would

enter: X, 2, +/-, INC SET.
d. Initiate the power feed move by pressing GO.
e. The feedrate is automatically set to 10 ipm (or 254 mm per min). Press FEED

or FEED

ê to adjust the feedrate from 1 ipm to 100 ipm. (or 25 to 2540)

é

40

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CN C Safety, P rogramming, Operating & Care Manual

f. Press STOP to halt power feed. Press GO to resume.

g. Repeat the process beginning at "c" above as often as you wish.
h. Press RETURN soft key to return to ma nual DRO operation.

6.5 Do One

The Do One routines in the DRO m ode allow you to do one CNC operation while
machining manually without having to write a program.

The programming and tool path of the events in Do One are nearly identical to those in
the Program Mode. See Section 8 for instructions for programming.

6.6 Go To (TRAKing/Electronic Handwheels Option)

The Go To function in the DRO mode allows you to set a dimension in X, Y or Z at which
you want the machine to st op moving when you are cranking manually. For example, if
you wanted to machine manually exactly 2" of table motion, you would input: Go To, X,
2, Inc Set. While the Go To window is displayed, the ProtoTRAK SMX will not let you
pass that 2" dimension you set.

a. Press the Go To key.
b. Enter the axis, X, Y, Z or any combination. Input the dimension(s).
c. Press Inc Set or Abs Set.
d. Crank the handwheel. Motion will stop at the enter ed dimension even if you continue

to crank the handwheel.

6.7 Teach

Teach gives you the ability to enter X and Y dimensions into a program. It can be a
useful way of entering a few manual moves for operations like clearing out excess
material or remembering a few hole locations.

The process of using Teach is in two parts. The first part takes place in the DRO Mode.
This is where you start the Teach program, establish the program events and enter the X
and Y dimensions. The second part is in the Program Mode. This is where you complete
the Teach events that you began in the DRO Mode by ente ring the rest of the data.
Once the data is entered, the Teach events become just like the other events that make
up a program.

6.7.1 Entering Teach Data

From the DRO screen, press Teach.
On the top of the screen, you will see the message "Teach" and an event counter. When

you enter Teach, you are actually programming events. If there is already a program in
current memory, Teaching will add events to the end of the program. If there is not
already a program in current memory, Teaching will start a new program. For example,
if you already had a program in current memory that had 10 events , when you press

41

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CN C Safety, P rogramming, Operating & Care Manual

Teach, the event counter will say EVENT 11. If there was no program, the event counter
will say EVENT 1.

The event counter shows the e vent for which data is being e ntered. You may teach in
position, drill and mill events only.

On the first Teach screen, the softkeys are:

POSN: a position move. For two-axis programming, the POSN and DRILL events are combined.
DRILL: a drill or bore.
MILL BEGIN: the beginning of a straight line or MILL event.
END TEACH: ends the teaching proces s and returns you to the main DRO screen.

If you press the POSN or DRILL key, the event counter will go up by one and the screen
remains the same. If you press the MILL BEGIN key, the event counter stays on the
same number. That is because you have given the beginning point of the line but not yet
the end. The softkey selections will change to:

MILL END: the last point of the Mill event. Press this to end the Mill event and select a
POSN, DRILL or new MILL e vent.

MILL CONT: the last point of the current Mill event, but the beginning of the next Mill
event. You may enter successive Mill events by pressing the MILL CONT key.

Pressing either of the above softkeys will cause the event counter to increase by one.

At any time you may exit the Teach and return to the DRO screen. The events you have
defined with their X and Y dimensions are finished in the Program Mode. See Section 8.14.

6.8 Return to Absolute Zero

At any time during manual DRO operation you may automatically move the table to your
absolute zero location in X and Y by pressing the RETURN ABS 0 soft key. When you
do, the message window will read "Ready to Begin: Press Go when Ready”. Make sure
your tool is clear and press the GO key. The servos will turn on, move the ram to Z
retract then move the table at rapid speed to your X and Y absolute zero position, and
then turn off. You will be at zero and in manual DRO operation. When you are in 2-axis
CNC operation, only the X and Y will move, the ram will not.

6.9 Spindle Operation (E-Head Option)

If the machine is equipped with the Programmable Electronic Head Option, spindle speeds
are set and adjusted through the SMX CNC. This feature became standard as of 1/1/11.

To set spindle speed press the SPIN SPEED softkey. The Data Input Line will prompt
“Spindle RPM”. Enter the RPM value (40-600 in low, 300-5000 in high) and press SET. If
the spindle was already on when you began to enter the new speed, it will stay at the
current speed until you press the SET key.

You may override the spindle speeds with the OVERRIDE display hard key. Press the F / S
key until the LED on the S (for Spindle) side is lit. Use the up and down arrow keys to
change the spindle speed in 5% increments per button press.

42

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CN C Safety, P rogramming, Operating & Care Manual

6.10 Tool #

The ProtoTRAK SMX CNC allows you to use the offsets for tools in your Tool Table (see
Section 11.1) in the DRO Mode. To chang e tools, press the TOOL # soft key and enter
the tool number when prompted by the Data Input Line.

Even when you set up a tool in the Set-Up Mode, if you do not wish to use the tools in the
Tool Table, simply ignore the Tool # feature.

.

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CN C Safety, P rogramming, Operating & Care Manual

43

7.2 The Program Mode header screen. Most selections above

Program Name and Dwell, The Advanced Features Option is not active.

7.0 Program Mode

Part 1: Getting Starte d & Some General Information

7.1 Programming Overview

The ProtoTRAK SMX CNC makes programming easy by allowing you to program the
actual part geometry as defined by the print.

The basic strategy is to first fill in the initial program information in the Program Header
screen and then program the features of the part by selecting the soft key event types
(geometry) and then fol low all instructions in the Data Input Line.

When an event is selected, all the prompts that need to be input will be shown on the
right side of the screen. The first prompt will be highlighted and also shown in the Data
Input Line. Input the dimension or data requested and press INC SET or ABS SET. For
X or Y dimension data it is very important to properly select INC SET or ABS SET. For
all other data either SET will do.

As data is being entered it will show in the Data Input Line. When SET, the data will be
transferred to the list of prompts in the right side of the screen, and the next prompt will
be shown in the Data Input Line.

When all data for an event has been entered, the entire event will be shifted to the left
side of the screen and the conversation line will ask you to select the next event.

7.2 Enter Program Mode

Press MODE, select PROGRAM soft key.
The ProtoTRAK SMX CNC will allow only one program in current memory. To write a new

program, you must first erase the one in current memory (you may want to first store the
program for use in the future ). If there is already a program in current memory, entering
the Program mode will allow you to edit or add to that program.

FIGURE

relate to the Advanced Features Option. If your screen shows only

.

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CN C Safety, P rogramming, Operating & Care Manual

44

FIGURE 7.3 Pressing the Help hard key when the Program Name is highlighted calls up alpha keys

7.3 Program Header Screen

The first screen you see when you enter the Program Mode is the Program Header
Screen. The Program Header Screen gives you options that apply to the entire program.
The softkey selections allow you to enter the program at any point.

The program name and general programming options you choose in the Program Header
Screen will be summarized in the program as "Event 0".

7.3.1 Program Name

Programs written on the ProtoTRAK SMX CNC are usually named for the part that is to be
machined. When programs (or files) are named us ing the ProtoTRAK SMX CNC, the
name can be up to 20 characters long. Programs imported into the ProtoTRAK SMX CNC
may be longer. While 20 characters are allowed, the entire program name may not be
shown in the status line or the program header screen.

Program names can include numbers, letters, spaces and other characters. When the
Program name prompt is highlighted, the Data Input Line will show "Program Name:". At
this point you may:

• Press number keys.

• Press Help to access alpha keys and special characters in the ProtoTRAK SMX

CNC.

• Use a keyboard plugged into the ProtoTRAK SMX CNC to name the program.

To use the alpha keys and special characters on the ProtoTRAK SMX CNC:
Use the Clear softkey to erase the entire line; the Backspace softkey to erase the last
character or number.

• Use the arrow softkeys to move around the table.

.

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CN C Safety, P rogramming, Operating & Care Manual

45

• Once the character you want is highlighted, use the Enter softkey to load the

character into the program name.

• Use the blank space on the lower right of the table to insert a space into the

program name.

• Once you finish entering the letters and special characters, press the End softkey.

This tells the ProtoTRAK SMX CNC that you are finished with the alpha table.
Numbers may still be added to the program name.

When you are finished with the program name, press SET to enter it into the current memory.

Note: It is not necessary to enter a part number. If none is entered and a GO TO soft key is
pushed, the system will assume a part number 0.

7.3.2 General Program Options

Use the DATA FWD softkey to select general programming options. See Section 3.1.2 for
more information about the Advanced Features O ption.

Scale: Allows a scale factor between .1 and 10. An input of 5 means the part will be 5
times as big as the programmed dimensions. A value of 1.0000 is assumed if nothing is
input. This function is part of the Advanced Features Option.

Dwell Request: Allows you to input a dwell at the bottom of a drill bolt hole or bore
cycle for events you select. Select the appropriate YES or NO soft key. If you select
YES you will be prompted to input a dwell time in seconds from .1 to 99.9 when
appropriate to the event being programmed.

Auxiliary Function Request: Asks if you wish to activate any of the optional auxiliary
functions (see Section 7.4) at any time during the program. Select the appropriate YES
or NO soft key. If you select YES you will be prompted to input the type and sequencing
of the auxiliary functions during event programming.

Event Comments: If you select "Yes" for event comments, you will have the
opportunity to insert a comment in each event. For Irregular Pocket and Irregular Profile
events, you will be able to enter a comment at the header event, but not for each A.G.E.
Turn and A.G.E. Arc event. This function is part of the Advanced Features Option.

Comments appear in the RUN mode on the Data Input Line as the event begins to run.
Comments may be composed of letters, numbers and some symbols and may be up to
20 characters.

While programming the event with the Event Comments set to Yes, when the highlight is
on the Event Comments prompt, you may enter a comment using the same methods
used to enter a program name, as described above.

Multiple Fixtures: Asks you if you wish to turn on the multiple fixtures offset.
Answering Yes will cause a prompt to appear at each event asking which fixture the
event was referenced from. If you select Yes, the Data Input Line will ask you to enter a
fixture default number from one to six. The fixture default number is the fixture that will
be applied to all the events in current memory when Multiple Fixtures is turned o n or
when a new event is programmed without another event being specified. Enter the
default fixture, or leave the number unchanged, and press SET. Multiple Fixtures are
explained more fully in Section 7.5. This function is part of the Advanced Features
Option.

Dimension Definition: The ProtoTRAK SMX CNC gives you a choice in programming either
tool path or geometry. Part Geometry programming allows you to define the geometry you
want your part to have and then the CNC does the difficult job of calculating tool path for

.

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CN C Safety, P rogramming, Operating & Care Manual

46

you automatically. This is a great benefit for most parts most of the time because it means
that the CNC is doing the hard work of determining tool position.

One restriction to part geometry programming is that for events to be connective, they
must lay on the same plane (see Section 5.3 for a definition of planes). For this reason,
the ProtoTRAK SMX CNC gives you the option of entering your own tool path. If you wish
to program the part by defining tool path yourself, you may choose the TOOL PATH
softkey. Otherwise, Part Geometry programming is assumed. Tool Path operates under
the same rules as standard RS274.

A program must be entirely written in Part Geometry or Tool Path programming, you
cannot combine the two methods in one program. Tool Path programming is part of the
Advanced Features Option.

7.3.3 Program Header Softkeys

The following softkeys are encountered in the Program Header Screen. The first five
listed below are always there. The last four appear when relevant to the general
programming option.

DATA FWD: moves the highlight forward through the programming opti ons without
setting an input into the p rogram.

DATA BACK: moves the highlight backwar d through the programming options without
setting an input into the p rogram.

GO TO BEGIN: puts the Program Header on the left side of the screen and the first
event on the right side.

GO TO END: puts the last programmed event on the left side of the screen and the next
event to be programmed on the right side.

GO TO #: enter the event number you wish to go to and then press SET. Puts the
requested event number on the right side of the screen and the previous event number
on the left.

Note: for a new program that has no Events, all the GO TO selections will take you to the
beginning, with the program header information summarized on the left (as Event 0) and the
Select an Event options for Event 1 on the right.

YES and NO: Yes and no appear when the Dwell Request, Auxiliary Funct ion Request
and the Event Comments are highlighted. Choosing Yes will give you prompts for using
these options while you are programming. You may return to the Program Header
Screen at any time to choose or cancel these prompts.

PART GEO: sets up the programming as Part Geometry.
TOOL PATH: sets up the programming as Tool Path. This function is part of the

Advanced Features Option.

7.4 Auxiliary (AUX) Functions

Auxiliary Functions are optional for the DPMSX2, DPMSX3, and DPMSX5, and s tandard for
the FHM5 and FHM7.

When the Auxiliary Function opti on is installed and active, the ProtoTRAK SMX CNC can
control four different auxiliary functions. You can select whethe r to activate or deactivate
these functions at the beginning or end of each event.

If Auxiliary Functions are selected on the program header, the system will prompt for
AUX BEG and AUX END in each event.

.

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CN C Safety, P rogramming, Operating & Care Manual

47

0

None

No Auxiliary functions will begin when this event begins to run.

3

Pulse Indexer

Activates a 0.3 second electronic pulse at the beginning of the event. See
0

None

No Auxiliary functions will turn off at the end of this event.

3

Pulse Indexer

Activates a 0.3 second electronic pulse at the end of this event. See note

When running programs with Auxiliary functions, the ACCESSORY hard key on the front panel
must be in the correct position. If you want the program to automatically turn the Auxiliary
functions on and off, press the ACCESSORY key until the light is on in the AUTO position.

AUX BEG Options:

Input: Function Comments

1 Coolant/Air The coolant pump or air solenoid will be turned on when this event begins to

AUX END Options:

1 Coolant/Air

Off

4 Spindle Turns off the spindle at the end of this event. Note, the spindle automatically

Coolant/Air on and off is automatically programmed for tool changes. If you want the air
or coolant pump on while cutting the entire part, you need only program the Aux be gin in
the first event and Aux end in the last event. The coolant pump or air solenoid will turn
on at the beginning of the programmed event and will turn off during tool changes.

The Pulse Indexer function is designed to operate with a standard indexer. Programming
an Aux 3 at the end of an event will cause the ProtoTRAK SMX CNC to stop machining at
the end of the event and wait for a signal from the indexer or rotary table that it has
finished its programmed move, then it will resume machining at the next event. If you
want the ProtoTRAK SMX CNC to return the head to the Z retract position before moving
to the next event, put the Aux 3 command in a Pause event. The ProtoTRAK SMX CNC
will interpret the signal from the indexer or rotary table as a GO command and continue
machining without you having to pr ess the GO key.

run.
note below.

Turns the coolant or air solenoid off at the end of this event.

below.
turns off for each tool change – it is not necessary to program a spindle off.

7.5 Multiple Fixtures

This function is part of the Advanced Features Option.
You may run your program using up to six fixtures plus a base. A fixture is a location on your

machine with a defined offset from your absolute 0. When you prog ram an event to have a
fixture, it will treat the offset as if it were absolute zero shift. The programmed X, Y and Z
absolute dimensions are relative to the absolute reference for the specified fixture.

For example, say you had two vises on the table. On the first vise, you established the
lower left jaw as the absolute 0. At the same time, you measured the distance between
the absolute zero you just established and the lower left jaw of the other vise. You
entered that measurement as an offset from your base vise (the first one) and the other
vise, which is Fixture #2. Any events that you programmed using Fix ture #2 would treat
the lower left corner of that second vise like the absolute 0 for the X, Y and Z dimensions
in the events.

Fixture offsets are handy for combining different programs together to run at the same
time or to make multiple parts by repeating the events with different fixtures.
The fixture offsets are entered in the Set-up mode. There is a base fixture, called fixture
number one. We recommend that Event #1 in your program uses fixture number one.
It doesn’t have to; we just believe it is clearer that way.

.

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CN C Safety, P rogramming, Operating & Care Manual

48

7.5.1 The Default Fixture

In the program header screen, you entered a default fixture number (if you didn’t, it assumed
fixture #1 as the default fixture). If there are program events already in current memory
when you change the multiple fixture from NO to YES, they will all receive the default fixture
number automatical ly. When you change the default fixture number in the program header
screen from one fixture to another, all the events that had the previous default fixture number
will be changed to the new default fixture number.

If there are no program events in current memory when you change the multiple fixture
feature from NO to YES, the prompt will be added to the end of every event you then
program. The default fixture number will be assumed if you press SET without specifying
a different numbe r. If you do specify a different fixture num ber that fixture number will
become the assumed input for subsequent events when SET is pressed.

7.5.2 Fixtures and Running the Program

To run the program, first go to the DRO mode and set absolute 0 at the base fixture,
Fixture #1.

In the Run mode, the SHOW ABS displays the absolute position relative to the fixture in
the event being run, that i s, the absolute dimension that was programmed.

7.5.3 Editing Fixtures

With the Multiple Fixtures feature turned to YES, you may edit the fixture number in the
Program Mode event by event. You may also use the Search Edit feature in the Edit
Mode to change fixture numbers.

See Section 11.4 for setting up fixt ure offsets.

7.6 Assumed Inputs

The ProtoTRAK SMX CNC will automatically program the following when you simply press
SET (either INC SET or ABS SET) :

Tool Offset: If the first event with an offset, CENTER. If not the first event with an
offset, the same as the last event if that event was a Mill or Arc event

Feedrate: same as last event if that event was a Mill, Arc, Pocket, Frame, or Helix
Tool #: same as last event, or Tool #1 if the first event
DRILL OR BORE: Drill
# PECKS FOR DRILL: 1 peck
CONRAD: 0

You may change these assumed inputs by simply inputting the desired data when the
event is programmed.

7.7 Z Rapid Positioning

Between any two events the head will always move to the higher of the Z rapid of the
event just completed or the Z Rapid of the next event, unless the two events are
connective (see Section 5.9). Remember, when using part geometry programming, two
milling events are not connective unless they lie in the same plane.

.

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CN C Safety, P rogramming, Operating & Care Manual

49

FIGURE 7.8 Soft keys used while programming an event

FIGURE 7.9.1 The header screen has been completed and is on the left side. Select an event type

from the soft keys

7.8 Softkeys within Events

Once a geometry (Event) such as Mill or Bolt Hole is selected, the softkeys will change.
See Figure 7.8

PAGE FWD :moves forward through the programmed events.
PAGE BACK: moves backwards through the programmed events.
DATA FWD: moves forward through the event inputs. Note, use the DATA FWD key and

not a SET key when you do not want to input a value.

DATA BACK: moves backwards through the event inputs.
DATA BOTTOM: puts the Highlight on the last input.
INSERT EVENT: use this to insert a new event into the program. This new event will

take the place of the one that was on the right side of the screen when you pressed the
INSERT EVENT key. That previous event, and all the events that follow, increase their
event number by one. For example, if you started with a program of four events, if you
were to press the INSERT EVENT key while Event 3 was on the right side of the screen,
the previous Event 3 would become Event 4 and the previous Event 4 would become
Event 5. If you insert a Subroutine event, the event numbers w ill increase by one as
when you insert another kind of event. If you insert a copy event, the event numbers
will increase by the number of events that are copied.

DELETE EVENT: this will delete the event on the right side of the screen.

7.9 Programming Events

Once you press the appropriate GO TO soft key, you will begin to define your part as a series of
Events. For the ProtoTRAK SMX CNC, an Event is a geometry, or a feature of a part.

.

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CN C Safety, P rogramming, Operating & Care Manual

50

7.9.2 When the More soft key is selected, these additional event types are available.

7.9.3 Here, a Bolt Hole event was selected. The ProtoTRAK SMX CNC

is prompting you to enter the number of holes.

When the MORE soft key is selected, the soft keys change to:

FIGURE

If the Advanced Features or E-Head Option are not active, relevant functions will be grayed out.

After an event type is selected from the soft keys, the prompts for that event will appear
on the right side of the screen. The data you need to enter to program the event will
appear in the Data Input Line. As soon as you enter one piece of data by pressing the
INC SET or ABS SET key, the next prompt will appear in the Data Input Line.

FIGURE

7.10 Editing Data While Programming

While programming an event, all data is entered by pressing the appropriate numeric
keys and pressing INC SET or ABS SET. If you enter an incorrect number before you
press INC SET or ABS SET you may clear the number by pressing RSTR (Restore).
Then, input the correct number and press SET.

If incorrect data has been entered and SET, you may correct it as long as you are still
programming that same event. Press the DATA BACK or DATA FWD (Forward) soft
key until the incorrect prompt and data are highlighted and shown in the conversation
line. Enter the correct number and SET. The ProtoTRAK SMX CNC will not allow you to
skip past prompts (by pressing DATA FWD) which need to be entered to complete an
event except when using the A.G.E. in the Irregular Pocket or Irregular Profile event.

Previous events may be edited by pressing the BACK hard key to the left of the soft keys.
The previous event will be shifted from the left side of the screen to the right and may be
edited. The BACK key may be pressed all the way to the Program Header Screen (the
PAGE BACK softkey will work as well).

.

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CN C Safety, P rogramming, Operating & Care Manual

51

7.11 LOOK

As you program each event, it is helpful to see your part drawn. For quick graphics while
in the Program Mode, press the LOOK hard key.

This function is active at the end o f each event, or whenever the co nversation line is
prompting Select Event. Press the LOOK key and the ProtoTRAK SMX CNC will draw the
part. Press LOOK again, or BACK to bring back the Select Event screen. You may also
select a new view or adjust the view.

Softkeys in LOOK:
ADJUST VIEW: gives additional options for adjusting the view of the drawing. See

below.
FIT DRAW: automatically resizes the drawing to fit the entire part program on the

screen.
LIST STEP: displays the list of events on the left side of the screen and with a purple

highlight on the first event. As LIST STEP is pushed, the highlight shifts to the next
event. As this happens, that event is also highlighted in the graphics by having its color
change to purple.

START EVENT NUMBER: will prompt you to enter an event number for highlighting.
This is useful for moving quickly to a particular event in a large program.

XY: displays a view in the XY plane.
YZ: displays a view in the YZ plane.
XZ: displays a view in the XZ plane.
3D: displays an isometric view

Softkeys in Adjust view:
FIT DRAW: automatically resizes the drawing to fit the entire part program on the screen.

6: shifts drawing down.
5: shifts drawing up.
3: shifts drawing to the left.
4: shifts drawing to the right.

ZOOM IN: makes the drawing larger.
ZOOM OUT: makes the drawing smaller.
RETURN: returns you to the first LOOK screen. The adjustments you made will stay on

the screen until you press ano ther selection that overrides those adjustments. The LIST
STEP function may be used with the adjustment unaltered.

Note: The LOOK routine does not check for programming errors. Use Tool Path in the SET UP
Mode to check movement of the tool.

.

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CN C Safety, P rogramming, Operating & Care Manual

52

7.13 Programming a Bolt Hole. On the left, the prompts required in programming in three-axis CNC.

On the right, the prompts required for two-axis.

7.12 Finish Cuts

The Pocket and Profile events are designed with built-in finish cut routines because they
are complete, and stand-alone pieces of geometry. Shapes machined with a series of Mill
or Arc events (either with or without A.G.E. Profile) don't have an automatic routine for
making finish cuts. There is, however, a very simple technique that can be used.

a. Program the shape using the print dimensions, and ignore the need to leave

material for a finish cut.

b. Using a subroutine e vent, Repeat all the events in "a." but call out a different tool

number.

c. In Set-Up Mode "lie" about the tool diameter for the tool called out in events in

"a.". Input a tool diameter equal to the actual tool diameter plus 2 times the finish
cut you wish to leave. The ProtoTRAK SMX CNC will think the tool is bigger than it
really is and, therefore, shift a little further away from the machined shape.

d. In Set-Up Mode input the actual diameter for the tool called in the Repeat event

"b". This will produce the final dimensioned cut.

7.13 Two Versus Three-Axis Programming

The ProtoTRAK SMX CNC may be operated as either a two or three-axis CNC. Many jobs
in tool rooms are simply easier to do with a two-axis CNC. Many jobs are more compl ex
or require a lot of metal removal, so the extra programming and set-up of the three-axis
is worth the effort.

The ProtoTRAK SMX CNC lets you choos e how much CNC you want to use on the job at
hand. See Section 4.6 for switching b etween two and thre e-axis operation.

Programming is very similar between the two.

FIGURE

EVENT 1 BOLT HOLE EVENT 1 BOLT HOLE

DRILL OR BORE # HOLES
# HOLES X CENTER
X CENTER Y CENTER
Y CENTER RADIUS
Z RAPID ANGLE
Z END TOOL #
RADIUS
ANGLE
# PECKS FOR DRILL
Z REEDRATE
TOOL #

In Figure 7.13 the prompts for programming a Bolt Hole in two-axis and in three-axis are
shown side by side. Note that the difference is that the three-axis requires a few
additional prompts.

.

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CN C Safety, P rogramming, Operating & Care Manual

53

Rather than duplicate needlessly, this manual will define all programming in three-axis.
This will serve to explain all issues in programming. For two-axis programming, some
event types and prompts do not appear.

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual

54

8.0 Program Mode

Part 2: Program Events

Events are fully defined pieces of geometry. By programming events, you tell the ProtoTRAK
SMX CNC what geometry you want to end up with; it figures the tool path for you from your
answers to the prompts and the tool information you give it in the Set-Up Mode.

8.1 POSN: Position Events

This event type positions the table and quill at a specified position. The positioning is
always at rapid speed (modified by feedrate override) and in the most direct path
possible from the previous location. The most common use of the position event is to
move the tool around an obstacle such as a clamp. For this reason, Z and X - Y motion
will not occur simultaneously. First, the Z (head) will move to the higher of the Z rapid
position of the current and next event, then the X (table) and Y (saddle) will move at to
the programmed position.

To program a Position event p ress the POSN soft key.
Prompts for the Position event:

X END is the X dimension to the position
Y END is the Y dimension to the position
Z Rapid is the Z dimension to the position
RPM is the spindle RPM for the event. INC SET will use the RPM of the previous event.

RPM Programming is not available for DPM SX2, SX3 or SX5 models that do not have the
Programmable Electronic Head Option.

Tool # is the tool number you assign. SET will use the tool number of the previous event.

8.2 DRILL Events

This event positions the table to the specified X and Y posit ion, moves the HEAD at rapid
to the Z RAPID location, feeds the quill to the Z END location, and rapids back to Z
RAPID for drill, and feeds back for bore.

Press the DRILL soft key.
Prompts for the drill event:

Drill=1, Bore=2: selects whether the hole is to be drilled or bored
X: is the X dimension to the hole
Y: is the Y dimension to the hole
Z Rapid: is the Z dimension to transition from rapid to feed
Z End: is the bottom of the hole
# PECKS: the factory setting is for each peck to be successively smaller, taking the

largest cuts at the beginning and the smallest at the end. When the highlight is on this
prompt, you may change this setting by pressing the HELP key. This will take you to a
screen where you may choose to have the same amount of material taken per peck.

RPM: is the spindle RPM for the event. INC SET will use the RPM of the previous event.
RPM Programming is not available for DPM SX2, SX3 or SX5 models that do not have the
Programmable Electronic Head Option.

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual

55

Z Feedrate: is the drilling feed r ate
Tool #: is the tool number you assign

8.3 BOLT HOLE Events

This event allows you to program a b olt hole pattern without needing to compute and
program the position of each hole.

Prompts for the Bolt Hole event:

Drill=1, Bore=2: selects whether the hole is to be drilled or bored
For the FHM5 and FHM7 and DPMs with the Programmable Electronic Head Option you

will also have the choice:

Tap = 3.
# Holes: is the number of holes in the bolt hole pattern
X Center: is the X dimension to the center of the hole pattern
Y Center: is the Y dimension to the center of the hole pattern
Z Rapid: is the Z dimension to transition from rapid to feed
Z End: is the bottom of the hole
Radius: is the radius of the hole pattern from the center to the center of the holes
Angle: is the angle from the positive X axes (that is, 3 o'clock) to any hole; positive angle is

measured counterclockwise from 0.000 to 359.999 degrees, negative angles measured clockwise.
Pitch: is the pitch of the tap that is used if the Tap option is chosen. Tap is available only if the

Programmable Electronic Head Option is active.
# PECKS: the factory setting is for each peck to be successively smaller, taking the

largest cuts at the beginning and the smallest at the end. When the highlight is on this
prompt, you may change this setting by pressing the HELP key. This will take you to a
screen where you may choose to have the same amount of material taken per peck.

RPM: is the spindle RPM for the event. INC SET will use the RPM of the previous event.
RPM Programming is not available for DPM SX2, S X3 or SX5 models that do not have the
Programmable Electronic Head Option.

Z Feedrate: is the drilling feed r ate
Tool #: is the tool number you assign

8.4 MILL Events

This event allows you to mill in a straight line from any one XYZ point to another, including
at a diagonal in space. It may be programmed with a CONRAD if it is connective with the
next event (this next event must lie in the same plane as the Mill event).

Prompts for the Mill event:

X Begin: is the X dimension to the beginning of the mill cut
Y Begin: is the Y dimension to the beginning of the mill cut
Z Rapid: is the Z dimension to transition from rapid to feed
Z Depth: is the depth of the cut in Z. If the Advanced Features option is active, Z

begin and Z end prompts will appear in place of Z depth.
Z Begin: is the Z dimension to the beginning of the mill cut (Advanced Fe atures option)

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual

56

X End: is the X dimension to the end of the mill cut; incremental is X Begin
Y End: is the Y dimension to the end of the mill cut; incremental is Y Begin
Z End: is the Z dimension to the end o f the mill cut; incremental is Z Begin (Advanced

Features option)
Conrad: is the dimension of a tangential radius to the next event (that must lie in the

same plane for part geometry programming)
Tool Offset: is the selection of the tool offset to right (input 1), offset to left (input 2),

or tool center--no offset (input 0) relative to the programmed edge and direction of tool
cutter movement and as projected in the XY plane.

RPM: is the spindle RPM for the event. INC SET will use the RPM of the previous event.
RPM Programming is not available for DPM SX2, SX3 or SX5 models that do not have the
Programmable Electronic Head Option.

Z Feedrate: is the Z feedrate from Z Rapid to Z begin
XYZ Feedrate: is the milling feedrate from Begin to End in in/min from .1 to 150, or

mm/min from 5 to 3810

Tool #: is the tool number you assign
Continue: Yes or no. This prompt appears when the Advanced Features Option is not

active in order to program a continuous tool path without stops and eliminate repetitive
prompts in the next event. If the Advanced Features Option is active, use the Profile
event to accomplish the same thing.

8.5 ARC Events

This event allows you to mill with circular contouring any arc (fraction of a circle) that lies
in the XY plane or a vertical plane (see Section 5.3). Vertical plane arcs are also limited
to those that are entirely concave or convex (in other words, if you think of the arc lying
on the surface of the earth, then it can't cross the equator).

In ARC events when X Center, Y Center, and Z Center are programmed incrementally,
they are referenced from X End, Y End, and Z End respectively. An ARC event may be
programmed with a CONRAD if it is connective with the next event (this next event must
lie in the same plane as the Arc event).

Note: When an arc is a 180o arc, there are several paths that all have the same beginning,
ending, and center locations. To illustrate, Imagine that if you were on the earth's equator and
you wanted to get to the other side of the earth you could go clockwise or counterclockwise
around the equator, or you could go up over the north pole, or down under the south pole. The
ProtoTRAK SMX CNC will automatically assume that all 180o arcs that have the same beginning,
ending and center dimensions for Z, lie in the XY plane. If you want a 180o arc in a vertical
plane, you must program two 90o arcs or some equivalent.

Prompts for the Arc event:

X Begin: is the X dimension to the beginning of the arc cut
Y Begin: is the Y dimension to the beginning of the arc cut
Z Rapid: is the Z dimension to transition from rapid to feed

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual

57

Z Depth: is the depth of the cut in Z. If the Advanced Features option is active, Z
begin and Z end prompts will appear in place of Z depth.

Z Begin: is the Z dimension to the beginning of the arc cut (Advanced Features option)
X End: is the X dimension to the end of the arc cut; incremental is from X Begin
Y End: is the Y dimension to the end of the arc cut; incremental is from Y Begin
Z End: is the Z dimension to the end of the arc cut; incremental is from Z Begin. The Z

End dimension is programmed only if the Advanced Features Option is active.

X Center: is the X dimension to the center of the arc; incremental is from X End
Y Center: is the Y dimension to the center of the arc; incremental is from Y End
Z Center: is the Z dimension to the center of the arc; incremental is from Z End. The Z

Center dimension is programmed only if the Advanced Features Option is active.
Conrad: is the dimension of a tangential radius to the next event (which mus t lie in the

same plane)
Direction: is the clockwise (input 1), or counterclockwise (input 2) direction of the arc

as viewed looking down for an arc in the XY plane,
plane, or looking from the right for a vertical YZ plane

looking from the front for a ver ti cal

Tool Offset: is the selection of the tool offset to right (input 1), offset to left (input 2),
or tool center--no offset (input 0) relative to the programmed edge and direction of tool
cutter movement and as projected in the XY plane

RPM: is the spindle RPM for the event. INC SET will use the RPM of the previous event.
RPM Programming is not available for DPM SX2, SX3 or SX5 models that do not have the
Programmable Electronic Head Option.

Z Feedrate: is the Z feedrate from Z Rapid to Z Begin
XYZ Feedrate: is the milling feedrate from Begin to End in in/min from .1 to 150, or

mm/min from 5 to 3810

Tool #: is the tool number you assign
Continue: Yes or no. This prompt appears when the Ad vanced Features Option is not

active in order to program a continuous tool path without stops and eliminate repetitive
prompts in the next event. If the Advanced Features Option is active, use the Profile
event to accomplish the same thing.

8.6 POCKET Event

This event selection gives you a choice between, circle pocket, rectangular pocket and
irregular pocket within the XY plane.

Pockets include machining the circumference, as well as all the material inside the
circumference of the programmed shape. If a finished cut is programmed, it will be
made at the completion of the final pass. The cutter wil l arc in and arc out of the finish
cut and position itself the finish cut dimension away from the part before moving the tool
out of the part.

The factory setting for tool stepover while machining a pocket is 70%. This may be
changed. When you first enter the pocket event, the blue ? will appear next to the help
key. Pressing Help will give you the choice of entering a new tool stepover percentage.
The value you enter here will remain the same until you change it again.

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual

58

8.6.1 Circular Pocket

Press the CIRCLE PCKT soft key if you wish to mill a circular pocket.
Prompts for the circle pocket:

X Center: is the X dimension to the center of the circle
Y Center: is the Y dimension to the center of the circle
Z Rapid: is the Z dimension to transition from rapid to feed
Z End: is the Z dimension at the bottom of the pocket; incremental is from the previous event
Radius: is the finish radiu s of the circle
Direction: is the clockwise (input 1), or counterclockwise (input 2) direction for milling
# Passes: number of cycles to machine to the final depth spaced equally from Z Rapid

to Z End (hint: keep Z Rapid small)
Entry mode: choose between a zigzag ramp and a plunge. The plung e will machine

straight down Z to the appropriate Z depth. The zigzag ramp will move in a zigzag
pattern to depth. See Section 8.6.5 for more information about the zigzag ramp.

Fin Cut: is the width of the finish cut. If 0 is input, the re will be no finish cut. See
Section 8.6.7 for a bottom f inis h cut.

RPM: is the spindle RPM for the event. INC SET will use the RPM of the previous event.
RPM Programming is not available for DPM SX2, SX3 or SX5 models that do not have the
Programmable Electronic Head Option.

FIN RPM: is the spindle RPM for the finish cut. FIN RPM programming is available with
the Programmable Electronic Head.

Z Feedrate: is the Z feedrate from Z rapid to Z end
XYZ Feedrate: is the milling feedrate in in/min from .1 to 150, or mm /min from 5 to 3810
Fin Feedrate: is the milling feedrate for the finish cut
Tool #: is the tool number you assign

8.6.2 Rectangular Pocket

Press RECTANGLE soft key if you wish to mill a rectangular pocket (all corners are 90o
right angles and the sides a r e parallel to the X and Y axes).

The prompts for the rectangular pocket:

X1: is the X dimension to any corner
Y1: is the Y dimension to the same corner as X1
X3: is the X dimension to the corner opposite X1; incremental is from X1
Y3: is the Y dimension to the same corner as X3; incremental is from Y1
Z Rapid: is the Z dimension to transition from rapid to feed
Z End: is the Z dimension at the bottom of the pocket; incremental is from the previous event

Conrad: is the value of the tangential radius in each corner
Direction: is the clockwise (input 1), or counterclockwise (input 2) direction for milling

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual

59

# Passes: is the number of cycles to machine to the final depth spaced equally from Z
Rapid to Z End (hint: keep Z Rapid small)

Entry mode: choose between a zig zag ramp and a plunge. The plunge will machine
straight down Z to the appropriate Z depth. The zigzag ramp will move in a zigzag
pattern to depth. See Section 8.6.5 for more information about the zigzag ramp.

Fin Cut: is the width of the finish cut. If 0 is input there will be no finish cut. See
Section 8.6.7 for a bottom f inis h cut.

RPM: is the spindle RPM for the event. INC SET will use the RPM of the previous event.
RPM Programming is not available for DPM SX2, S X3 or SX5 models that do not have the
Programmable Electronic Head Option.

FIN RPM: is the spindle RPM for the finish cut. FIN RPM programming is available with
the Programmable Electronic Head.

Z Feedrate: is the Z feedrate from Z rapid to Z end
XYZ Feedrate: is the milling feedrate in in/min from .1 to 150, or mm/min from 5 to 3810
Fin Feedrate: is the milling feedrate for the finish cut
Tool #: is the tool number you assign

8.6.3 Irregular Pocket (Advanced Features Option)

Press the IRREG PCKT soft key if you wish to mill a pocket other than a rectangle or
circle. The Irregular Pocket event gives you the powerful Auto Geometry Engine to
define a shape made up of straight lines (Mills) and arcs.

The first screen in an irregular pocket event will define the beginning point and some of
its general parameters. The last event of the irregular pocket must end at the same
point as defined in the first event.

X Begin: is the X dimension of the beginning of the pocket
Y Begin: is the Y dimension of the begin ning of the pocket
Z Rapid: is the Z dimension to transition from rapid to feed
Z End: is the Z dimension of the depth of the pocket.
# Passes: is the number of cycles to machine to the final depth spaced equally

from Z rapid to Z end (hint: keep Z Rapid small)
Entry mode: choose between a zig zag ramp and a plunge. The plunge will machine

straight down Z to the appropriate Z depth. The zigzag ramp will move in a zigzag
pattern to depth. See Section 8.6.5 for more information about the zigzag ramp.

Z Feedrate: is the Z feedrate from Z rapid to Z end
XYZ Feedrate: is the milling feedrate in in/min from .1 to 150, or mm/min from 5 to 3810
Fin Cut: is the width of the finish cut. If 0 is input there will be no finish cut. See

Section 8.6.7 for a bottom f inish cut.
RPM: is the spindle RPM for the event. INC SET will use the RPM of the previous event.

RPM Programming is not available for DPM SX2, SX3 or SX5 models that do not have the
Programmable Electronic Head Option.

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual

60

FIN RPM: is the spindle RPM for the finish cut. FIN RPM programming is available with
the Programmable Electronic Head.

Fin Feedrate: is the finish cut milling feedrate in in/min from .1 to 150, or mm/min
from 5 to 3810

Tool #: is the tool number you assign
When the initial screen is complete, you will define the perimeter of the pocket with a

series of A.G.E. Mills and A.G.E. Arcs. Programming with the Auto Geometry Engine is
explained in Sectio n 9.0.

No islands may exist in an irregular pocket.

8.6.4 Tool Path in Pocket Events

In Program Run, the p ocket path will be either the plunge or zigzag cuts to Z depth along
either the X or Y, followed by the required number of cuts to clear out the interior
material, and the n the rough cut along the inside of the perimeter. This will be repeated
for each pass and then followed by a finish pass (if FIN CUT was not zero) along the
inside of the perimeter at the Finish Feedrate and final depth. If a bottom finish cut was
programmed, it will be machined before the perimeter finish cut.

Whether the cuts to clear the interior material of the irregular pocket are along the X or
Y-axis depends on if there are hidden areas of the pocket. The ProtoTRAK SMX CNC
always looks to cut along the X-axis first. If there are areas that are hidden to the X­axis, it will machine along the Y-axis. I f there are hidden areas that cannot be machined
continuously in the X or Y-axis, the tool will return to Z retract and then reposition to
machine the hidden a rea.

8.6.5 Zigzag Z Depth Cuts

In programming pocket events, you have a choice to program the cuts to Z depth either
as a plunge or a zigzag ramp. For rectangular and circular pockets, the tool will start in
the center of the pocket. For irregular pockets, since there is no center defined, the tool
will start in the lower left corner of the pocket. The direction of the ramp will be the
same as the initial direction in either X or Y, depending on how the pocket is to be cut.

The tool will zigza g back and forth along the X or Y over a length of one tool radius while
at the same time moving in the Z direction. When it tra vels one tool radius along this
direction, it will have traveled a distance of ten percent of the tool diameter along the Z.
This works out to roughly ramping into t he part at an angle of 11 degrees.

In order to use a zigzag ramp, the X or Y move must be larger than the diameter of the
tool plus the radius of the tool, minus the finish cut of the pocket. The formula is:

the pocket x or y move > tool diameter + tool radius - fin cut

If the tool is too large for the zigzag ramp, the ProtoTRAK SMX CNC will give an error message
during program run and will then default to plunge. This will occur for eac h pass of the pocket
depth.

8.6.6 Conrad in Pocket Events

A Conrad may be added to the last event of an Irregular Pocket. The Conrad will be inserted
between the end of the last event and the beginning of the next event.

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual

61

8.6.7 Bottom Finish Cut

The standard finis h cut is along the walls of the part, but you may have the ProtoTRAK
machine a finish cut along the bottom as well. When the highlight is on the Fin Cut
prompt, the blue ? appears next to the Help key. Pressing help gives you the ability to
choose a Finish cut in Z. You can remove t he bottom finish cut by placing the highlight
on the Fin Cut prompt and pressing Help again. When you s elect Yes to the bottom
finish cut, the following prompt will appear:

Z FIN CUT: the finish cut at the bottom.

8.6.8 Face Mill (Advanced Features Option)

Press Face Mill soft key if you wish to face or clean up the top of a workpiece.
The cutter will automatically start off of the part that you define. The cutter will move

along the X axis to remove the material starting from where you defined X1, Y1 and
finishing at the corner programmed as X3, Y3.

The prompts for the face mill:

X1: is the X dimension to any corner
Y1: is the Y dimension to the same corner as X1
X3: is the X dimension to the corner opposite X1; incremental is from X1
Y3: is the Y dimension to the same corner as X3; incremental is from Y1
Z Rapid: is the Z dimension to transition from rapid to feed
Z End: is the Z dimension at the bottom of the pocket; incremental is from the previous

event
# Passes: is the number of cycles to machine to the final depth spaced equally from Z

Rapid to Z End.

Z Fin Cut: is the depth of the finish cut. If 0 is input t here will be no finish cut.
RPM: is the spindle RPM for the event. INC SET will use the RPM of the previous event.
FIN RPM: is the spi ndle RPM for the finish cut.
Z Feedrate: is the Z feedrate from Z rapid to Z end in in/min from .1 to 700, or

mm/min from 5 to 17780
XYZ Feedrate: is the milling feedrate in in/min from .1 to 800, or mm/min from 5 to

20320

Fin Feedrate: is the milling feedrate for the finish cut
Tool #: is the tool number you assign

Note – if you press the HELP key when you are on the X1 prompt, you can adjust the
step over distance of the face mill. The default is 95% of the cutter width. You can
adjust it from 1 to 99%.

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual

62

8.7 Islands (Advanced Features Option)

Islands programming is available as part of the Advanced Features Option. See Section

3.1.2.
Within the Pocket event choices, you may also sele ct a circular, rectangular or irregular

island. An island is a shape that is left standing when the surrounding material is
removed. The ProtoTRAK gives you the ability to machine almost any shape as an island
within a rectangular pocket. Both the shape of the island and the dimension of the
surrounding pocke t are defined within the island event.

The tool path for machining the island event is that the tool will first plunge or ramp into
the material next to the island, offset by the programmed finish cut, to the depth of the
first pass. The tool will machine the perimete r of the island, offset by the island finish
cut. Then the tool will machine the material in the pocket in a spiral path, moving away
from the island in the programmed clockwise or co unterclockwise direction. It will
continue this outward spiral motion until it encounters the programmed rectangular
perimeter (or pocket). It will then follow the perimeter, offset by the pocket finish cut.

It will proceed in this manner through the number of programmed passes. On the final
pass, it will machine the island finish cut, then the pocket finish cut. If a Z finish cut is
programmed, it will do this in the same spiral pattern as the roughing passes between
machining the island and pocket finish cuts. The tool will ramp away from the finish cut
by the amount of the finish cut before it raises out of the part.

8.7.1 Circular Island (Advanced Features Option)

Press the Circle Island soft key if you wish to mill a circular island.
Prompts for the Circle Pocket:

X CENTER: is the dimension of the center of the Island
Y CENTER: is the dimension of the center of the Island
Z RAPID: is the Z dimension of the transition from rapid to feed
Z END: is the Z dimension at the bottom of the pocket; incremental is from the previous event
RADIUS: is the finish radius of the Island
DIRECTION: is the milling direction, clockwise or counterclockwise
#PASSES: the number of roughing passes to the depth
ENTRY MODE: choose between zigzag ramp and plunge. The plunge will machine

straight down Z to the appropriate Z depth. The zigzag ramp will move in a zigzag
pattern to depth. See the previous section for more information about the zigzag ramp.

FIN CUT ISL: Finish cut for the Island. If 0 is input, there will be no finish cut. See the
previous section for a bottom finish cut.

X1 POCKET: X dimension for one corner of the rectangular pocket that surrounds the island.
Y1 POCKET: Y dimension for one co rner of the rectangular pocket that surrounds the isl and.

X3 POCKET: X dimension for the opposite corner of the rectangular pocket that

surrounds the island.
Y3 POCKET: Y dimension for the opposite corner o f the rectangular pocket that

surrounds the island.

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual

63

CONRAD PCKT: the value of the tangential radius in the corners of the rectangular
pocket that surrounds the island.

FIN CUT PCKT: finish cut along the perimeter of the pocket. If 0 is input, there will be
no finish cut. See the previous section for a bottom finish cut.

RPM is the spindle RPM for the event. INC SET will use the RPM of the previous event.
RPM Programming is not available for DPM SX2, S X3 or SX5 models that do not have the
Programmable Electronic Head Option.

FIN RPM: is the spindle RPM for the finish cut. FIN RPM programming is available with
the Programmable Electronic Head.

Z FEEDRATE: is the Z feedrate from Z rapid to Z end.
XYZ FEEDRATE: the milling feedrate in in/min from .1 to 150, or mm/min from 5 to 3810
FIN FEEDRATE: the finish milling feedrate for both the island and pocket finish cuts
TOOL #: is the tool number you assign.

8.7.2 Rectangular Island (Advanced Features Option)

Press the RECT ISLAND softkey if you wish to machine a rectangular island.
Prompts for the RECT ISLAND:

X1 ISLAND: X dimension for one corner of the rectangular island.
Y1 ISLAND: Y dimension for one corner of the rectangular island.
X3 ISLAND: X dimension for the opposite corner of the island.
Y3 ISLAND: Y dimension for the opposite corner of the island.
Z RAPID: is the Z dimension of the transition from rapid to feed
Z END: is the Z dimension at the bottom of the pocket; incremental is from the previous event
CONRAD ISL: the value of the tangential radius in the corners of the island.
DIRECTION: is the milling direction, clockwise or counterclockwise
#PASSES: the number of roughing passes to the depth
ENTRY MODE: choose between zigzag ramp and plunge. The plunge will machine

straight down Z to the appropriate Z depth. The zigzag ramp will move in a zigzag
pattern to depth. See the previous section for more information about the zigzag ramp.

FIN CUT ISL: Finish cut for the Island. If 0 is input, there will be no finish cut. See the
previous section for a bottom finish cut.

X1 POCKET: X dimension for one corner of the rectangular pocket that surrounds the island.
Y1 POCKET: Y dimension for one co rner of the rectangular pocket that surrounds the isl and.
X3 POCKET: X dimension for the opposite corner of the rectangular pocket that

surrounds the island.
Y3 POCKET: Y dimension for the opposite corner o f the rectangular pocket that

surrounds the island.
CONRAD PCKT: the value of the tangential radius in the corners o f the rectangul ar

pocket that surrounds the island.

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual

64

RPM: is the spindle RPM for the event. INC SET will use the RPM of the previous event.
RPM Programming is not available for DPM SX2, SX3 or SX5 models that do not have the
Programmable Electronic Head Option.

FIN RPM: is the spindle RPM for the finish cut. FIN RPM programming is available with
the Programmable Electronic Head.

FIN CUT PCKT: finish cut along the perimeter of the pocket. If 0 is input, there will be
no finish cut. See the previous section for a bottom finish cut.

Z FEEDRATE: is the Z feedrate from Z rapid to Z end.
XYZ FEEDRATE: the milling feedrate in in/min from .1 to 150, or mm/min from 5 to 3810
FIN FEEDRATE: the finish milling feedrate for both the island and pocket finish cuts
TOOL #: is the tool number you assign.

8.7.3 Irregular Island (Advanced Features Option)

Press the IRREG ISLAND key if you wish to mill an island other than a rectangle or circle.
The Irregular Island gives you the powerful Auto Geometry Engine to define a shape
made up of straight lines and arcs.

The first screen in an Irregular Island event will de fine the beginning point and some of
its general parameters. The last event of the irregular pocket must end at the same
point as defined in the first event.

Prompts for the Irregular Island event:

X BEGIN: X dimension t o the beginning of t he island.
Y BEGIN: Y dimension to the beginning of the island.
Z RAPID: is the Z dimension of the transition from rapid to feed
Z END: is the Z dimension at the bottom of the pocket; incremental is from the previous event
#PASSES: the number of roughing passes to the depth
ENTRY MODE: choose between zigzag ramp and plunge. The plunge will machine

straight down Z to the appropriate Z depth. The zigzag ramp will move in a zigzag
pattern to depth. See the previous section for more information about the zigzag ramp.

FIN CUT ISL: Finish cut for the Island. If 0 is input, there will be no finish cut. See the
previous section for a bottom finish cut.

X1 POCKET: X dimension for one corner of the rectangular pocket that surrounds the island.
Y1 POCKET: Y dimension for one co rner of the rectangular pocket that surrounds the isl and.
X3 POCKET: X dimension for the opposite corner of the rectangular pocket that

surrounds the island.
Y3 POCKET: Y dimension for the opposite corner of the rectangular pocket that

surrounds the island.
CONRAD PCKT: the value of the tangential radius in the corners of the rectangular

pocket that surrounds the island.
FIN CUT PCKT: finish cut along the perimeter of the pocket. If 0 is input, there will be

no finish cut. See the previous section for a bottom finish cut.

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual

65

RPM: is the spindle RPM for the event. INC SET will use the RPM of the previous event.
RPM Programming is not available for DPM SX2, S X3 or SX5 models that do not have the
Programmable Electronic Head Option.

FIN RPM: is the spindle RPM for the finish cut. FIN RPM programming is available with
the Programmable Electronic Head.

Z FEEDRATE: is the Z feedrate from Z rapid to Z end.
XYZ FEEDRATE: the milling feedrate in in/min from .1 to 150, or mm/min from 5 to 3810.
FIN FEEDRATE: the finish milling feedrate for both the island and pocket finish cuts.
TOOL #: is the tool number you assign.

When the initial screen is complete, you will define the perimeter of the island with a
series of A.G.E. Mills and A.G.E. Arcs. Programming with the Auto Geometry Engine is
explained in Sectio n 9.0.

8.8 PROFILE Events

This event allows you to mill around the outside or inside of a circular or rectangular frame or an
irregular profile. The irregular profile may be closed or open. All profiles are limited to the XY plane.

When the irregular profile event is started the ProtoTRAK SMX CNC will automatically initiate the
powerful Auto Geo metry Engine. See Section 9.0 for pr ogramming with A.G.E.

8.8.1 Circle profile

Press the CIRCLE soft key if you wish to mill a circular frame.
Prompts in the Circle Profile event:

X Center: is the X dimension to the center of the circle
Y Center: is the Y dimension to the center of the circle
Z Rapid: is the Z dimension to transition from rapid to feed
Z End: is the Z dimension to the bottom of the frame; incremental is from the previous event
Radius: is the finish radiu s of the circle
Direction: is the clockwise (input 1), or counterclockwise (input 2) direction for milling
Tool Offset: is the selection of the tool offset to the right (input 1), offset to the left

(input 2), or tool center--no offset (input 0) relative to the programmed edge and
direction of the cutter movement

# Passes: is the number of cycles to machine to the final depth spaced equally from Z
Rapid to Z End (hint: keep Z Rapid small)

Fin Cut: is the width of the finish cut. If 0 is input, there will be no finish cut
RPM: is the spindle RPM for the event. INC SET will use the RPM of the previous event.

RPM Programming is not available for DPM SX2, SX3 or SX5 models that do not have the
Programmable Electronic Head Option.

FIN RPM: is the spindle RPM for the finish cut. FIN RPM programming is available with
the Programmable Electronic Head.

Z Feedrate: is the Z feedrate from Z rapid to Z end
XYZ Feedrate: is the milling feedrate in in/min from .1 to 150, or mm/min from 5 to 3810

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual

66

Finish Feedrate: is the milling feedrate for the finish cut
Tool #: is the tool number you assign

8.8.2 Rectangular Profile

Press the RECTANGLE soft key if you wish to mill a rectangular frame (all corners are
90o right angles).

Prompts for the rectangular profile:

X1: is the X dimension to any corner
Y1: is the Y dimension to the same corner as X1
X3: is the X dimension to the corner opposite X1; incremental is from X1
Y3: is the Y dimension to the same corner as X3; incremental is from Y1
Z Rapid: is the Z dimension to transition from rapid to feed
Z End: is the Z dimension at the bottom of the frame; incremental is from the previous event
Conrad: is the value of the tangential radius in each corner
Direction: is the clockwise (input 1), or counterclockwise (input 2) direction for milling
Tool Offset: is the selection of the tool offset to the right (input 1), offset to the left

(input 2), or tool center--no offset (input 0) relative to the programmed edge and
direction of the cutter movement

# Passes: is the number of cycles to machine to the final depth spaced equally from Z
Rapid to Z End (hint: keep Z Rapid small)

Fin Cut: is the width of the finish cut. If 0 is input, there will be no finish cut
RPM: is the spindle RPM for the event. INC SET will use the RPM of the previous event.

RPM Programming is not available for DPM SX2, SX3 or SX5 models that do not have the
Programmable Electronic Head Option.

FIN RPM: is the spindle RPM for the finish cut. FIN RPM programming is available with
the Programmable Electronic Head.

Z Feedrate: is the Z feedrate from Z rapid to Z end
XYZ Feedrate: is the milling feedrate in in/min from .1 to 150, or mm/min from 5 to 3810
Fin Feedrate: is the milling feedrate for the finish cut (if programmed).
Tool #: is the tool number you assign

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual

67

8.8.3 Irregular Profile (Advanced Features Option)

Press the IRREG PROFILE soft key if you wish to mill a profile other than a rectangle or
circle. The Irregular Profile event gives you the powerful Auto Geometry Engine to
define a shape made up of straight lines (Mills) and arcs.

The Irregular Profile is a series of events that are programmed to machine continuously.
The first event of the series will be called an IRR PROFILE and it will define the beginning
point of the profile and other information that applies to the entire profile.

X Begin: is the X dimension of the beginning of the profile
Y Begin: is the Y dimension of the beginning of the profile
Z Rapid: is the Z dimension to transition from rapid to feed
Z End: is the Z dimension of the depth of the profile
Tool Offset: is the selection of the tool offset to right (input 1), offset to left (input 2), or tool

center--no offset (input 0) relative to the programmed edge and direction of tool cutter movement
# Passes: is the number of cycles to machine to the final depth spaced equally from Z

rapid to Z end (hint: keep Z Rapid small)

Z Feedrate: is the Z feedrate from Z rapid to Z end
XYZ Feedrate: is the milling feedrate in in/min from .1 to 150, or mm/min from 5 to 3810
Fin Cut: is the width of the finish cut. If 0 is input there will be no finish cut
RPM: is the spindle RPM for the event. INC SET will use the RPM of the previous event.

RPM Programming is not available for DPM SX2, SX3 or SX5 models that do not have the
Programmable Electronic Head Option.

FIN RPM: is the spindle RPM for the finish cut. FIN RPM programming is available with
the Programmable Electronic Head.

Fin Feedrate: is the finish cut milling feedrate in in/min from .1 to 150, or mm/min
from 5 to 3810

Tool #: is the tool number you assign
When the initial Irregular Profile screen is complete, the rest of the profile is programmed

using A.G.E. Mill and A.G.E. Arc events. Programming with the Auto Geometry Engine is
explained in Sectio n 9.0.

8.9 Helix Events (Advanced Features Option)

The Helix Event is found after you press the MORE softkey from the Select Event screen.
It allows you to machine in a circular path in the XY plane while you simultaneously
move the Z-axis linearly.

Press the HELIX soft key.

X Center: is the X dimension to the center of rotation of the helix
Y Center: is the Y dimension to the center of rotation of the helix
Z Rapid: is the Z dimension to transition from rapid to feed
Z Begin: is the Z dimension to the beginning of the helix
Z End: is the Z dimension at the end of the helix
Radius: is the radius from the center of rotation to the helix

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual

68

Angle: is the angle from the positive X axis (that is, 3 o'clock) to the starting position of the helix
# Rev: is the number of revolutions in the helix, for example, 0.75 would be

270 degrees, or 3.25 would be three times around plus 90 degrees

Direction: is the clockwise (input 1) or counterclockwise (input 2) direction of t he helix
Tool Offset: is the selection of the tool offset to right (input 1), offset to left (input 2),

or tool center--no offset (input 0) relative to the programmed edge and direction of the
cutter movement

RPM: is the spindle RPM for the event. INC SET will use the RPM of the previous event.
RPM Programming is not available for DPM SX2, S X3 or SX5 models that do not have the
Programmable Electronic Head Option.

XYZ Feedrate: is the feedrate from beginning to end in in/min from .1 to 150, or
mm/min from 5 to 3810

Tool #: is the tool you assign

8.10 Subroutine Events

The Subroutine Events are used for ma nipulating previously programmed geometry
within the XY plane.

The Subroutine Event is divided into three options: Repeat, Mirror, and Rotate.
Repeat and Rotate may be connective. As long as the rules of connectivity are satisfied

(see Section 5.9), the ProtoTRAK SMX CNC will continue milling between preceding and
subsequent events.

REPEAT allows you to repeat an event or a group of events up to 99 times with an
offset in X and/or Y and/or Z. This can be useful for drilling a series of evenly spaced
holes, duplicating some machined shapes, or even repeating an entire program with an
offset for a second fixture.

Repeat events may be "nested." That is, you can repeat a repeat event, of a repeat event, of
some programmed event(s). One new tool number may be assigned for each Repeat Event.

MIRROR (Advanced Features Option) is used for parts that have symmetrical
patterns or mirror image patterns. In addition to specifying the events to be repeated,
you must also indicate the axis or axes (X or Y or XY are allowed) that the reflection is
mirrored across. In addition, you must specify the of fset from absolute zero to the line
of reflection. You may not mirror another mirror event, or mirror a rotate event.
Consider the figure below:

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual

69

8.10.1 Holes 1-4 are mirrored across the Y axis to 5-8, respectively, about a line X OFFSET from

X=absolute 0

FIGURE 8.10.2 Shape A programmed with 4 MILL events and Conrads. Using ROTATE, these 4 events are rotated

through a 45 degree angle about a point offset from absolute zero by X Center and Y Center

dimensions. A is rotated 3 times to produce shape B, C, and D

FIGURE

ROTATE is used for polar rotation of parts that have a rotational symmetry around some
point in the XY plane. In addition to specifying the events to be repeated, you must also
indicate the absolute X and Y position of the center of rotation, the angle of rotation
(measured counterclockwise as positive; and clockwise as negative), and the number of
times the specified events are to be rotated and repeated. You may not rotate another
rotate event, however you can rotate a mirror event. Consider the figure below:

Press the SUBROUTINE (SUB) soft key to call up the Repeat, Mirror, and Rotate options.

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual

70

8.10.1 Repeat

Press the REPEAT soft key .
Where:

First Event #: is the event number of the first event to be repeated
Last Event #: is the event number of the last event to be repeated; if only one event is

to be repeated, the Last Event # is the same as the First Event #

X Offset: is the incremental X offset from event to be repeated
Y Offset: is the incremental Y offset from event to be repeated
Z Offset: is the incremental Z offset from event to be repeated
Z Rapid Offset: is the incremental Z rapid offset from event to be repeated
# Repeats: is the number of times events are to be repeated up to 99
% RPM: is the percentage of RPM in the programmed events. SET will load in the

assumed % of 100%. RPM Programming is not available for DPM SX2, SX3 or SX5
models that do not have the Programmable Electronic Head Option.

% Feed: the percentage of the feeds programmed in the repeated events. 100% is
assumed

Tool #: is the tool number you assign

8.10.2 Mirror (Advanced Features Option)

Press the MIRROR soft key.

First Event #: is the event number of the first event to be mirrored
Last Event #: is the event number of the last event to be mirrored; if only one event is

to be mirrored, the last event is the same as the first.
Cutting Order: input 1 to cut from the lowest mirrored event to the highest (forward)

and 2 to machine from the highest mirrored event to the lowest (backward).
This way you can keep all the machine motion in a consistent direction as it moves from
the original shape to the mirrored shape and keep all cutting either climb or
conventional.

Mirror Axis: is the selection of the axis or axes to be mi rrored (input X or Y or XY, SET)
X Offset: is the distance from Y absolute 0 to the Y-axis line of reflection
Y Offset: is the distance from X absolute 0 to the X-axis line of reflection

8.10.3 Rotate

Press the ROTATE soft key.
First Event #: is the event number of the first event to be rotated
Last Event #: is the event number of the last event to be rotated; if only one event is

to be rotated, the last event is the same as the first
X Center: is the X absolute position of the center of rotation

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual

71

Y Center: is the Y absolute position of the center of rotation
Angle: is the angle of rotation of the repeated events (positive is counterclockwise;

negative is clo c kwise)

# Repeats: is the number of times events are to be rotated up to 99

8.11 COPY Events (Advanced Features Option)

Copy Events are programmed exactly like Subroutine Events. The only difference is that
in Copy the events are rewritten into subsequent events. If, for example, in event 11
you Copy Repeated events 6, 7, 8, 9, 10 with 2 repeats, events 6-10 would be copied
with the input offsets into events 1 1-15, and recopied into 16-20.

Copy Events may be Repeat, Mirror , Rotate or Drill to Tap.
Copy is very use ful. With Copy you can:

• Edit the events that are being repeated, mirrored or rotated without changing the
original events.

• Co nnect so that the quill will not move up to the Z Rapid position, and back down
unnecessarily. However, to be connective, you must be certain that the X, Y, Z
begin of the first event, once offset or rotated, coincides with the X, Y, Z end of the
last event.

• Program an event parallel to X or Y (where the geometry is the easiest to
describe), rotate it to the desired position, then delete the original.

• Use the Clipboard to paste previously stored events from another program into the

current program. After you press the Clipboard key, you will enter the offset from
the previous program's absolute zero to the current program's absolute zero (see
figure below). For information about putting events into the clipboard, see Section

10.4.

Figure 8.11 In the above example, the offset that puts the group of holes in the desired
location is X=-1.50 and Y=-1.00.

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual

72

8.11.1 Copy Drill to Tap

The copy drill to tap feature allows you to convert a series of drill events over to a tap
event. Prompts in this event.

First Event #: is the event number of the first drill event to be copied
Last Event #: is the event number of the last drill event to be repeated; if only one

event is to be repeated, the Last Event # is the same as the First Event #
Z Rapid: is the Z dimension to transition from rapid to feed. Make sure that Z rapid is

set high enough to compensate for the amount of float in the floating tapping head.

Z End: the depth of the thread
PITCH - the distance from one thread to the next in inches or mm. It is equal to one

divided by the number of threads per inch. For example, the pitch for a 1/4-20 screw is
1 ÷ 20 = .05 inches

RPM: spindle RPM
Tool #: is the tool number you assign

8.12 Thread Mill Event (Advanced Features Option)

To program a Thread Mill event press the Thread mill soft key. This event includes an
automatic move in and out by 0.050” of the thread. Prompts in the Thread Mill event:

X CENTER: the X dimension of the center of the thread
Y CENTER: the Y dimension of the center of the thread
Z RAPID: the Z dimension where the Z rapid feed slows to Z program feed
Z BEGIN: the Z dimension where the thre ading pass begins
Z END: the Z bottom of the thread
PITCH: the distance from one thread to the next in inches or mm. It is equal to one

divided by the number of threads per inch. For example, the pitch for a 1/4-20 screw is
1 ÷ 20 = .05 inches

MAJOR DIA: the largest diameter of the thread (the root for an ID thread, the crest for
an OD thread)

MINOR DIA: the smallest diameter of the thread (the root for an OD thread, the crest
for an ID thread)

SIDE: input 1 for inside, 2 for outside
ANGLE: the angle the tool feeds into the beg inning depth
DIRECTION: clockwise or counterclockwise
# PASSES: - the number of passes to cut the thread to its final dept h
Z FEEDRATE: The feedrate from Z Rapid to Z Begin
XYZ FEEDRATE: The feedrate of XYZ along the path of the helix.

FIN CUT: width of the finish cut. If 0 is input, there is no finish cut.

If something other than 0 is input for finish cut, the following prompt appears:

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual

73

FIN FEEDRATE: the milling feedrate for the finish cut.
RPM: is the spindle RPM for the event. INC SET will use the RPM of the previous event.

RPM Programming is not available for DPM SX2, SX3 or SX5 models that do not have the
Programmable Electronic Head Option.

FIN RPM: is the spindle RPM for the finish cut. FIN RPM programming is available with
the Programmable Electronic Head.

TOOL#: is the tool number you assign.

8.13 PAUSE Events

The purpose of the Pause Event is to allow you to progra m a stop condition within the
program. The effect of this event is to turn off the spindle, move the head to the Z
retract location with the X and Y position corresponding to the end of the previous event
and stopping the program run.

Pause events are useful if you want to stop the program to make a measurement,
change a fixture, et c.

NOTE: In general, you should avoid programming a PAUSE event between two connective
events. The Pause event will cause the events to NOT be connective.

To program a Pause Event press the PAUSE soft key. Because there is no input
required, simply press SET to load a nd the event counter will advance by one and the
Select Event screen will reappear.

In run, press the GO key after a pause to continue.

8.14 Tap Events (Programmable Electronic Head)

Tap events allow you to tap holes using a floating tapping head. The feedrate of the
thread will be calculated from the pitch and RPM entered. The RPM range that the
ProtoTRAK SMX can tap for low gear is 40 to 200 RPM and for high gear is 300 to 1000
RPM. An error message will occur if you try to tap outside of these ranges.

To program a tap event press the TAP soft key.
Prompts in the Tap event:

X: the X dimension to the center of the hole
Y: the Y dimension to the center of the hole
Z Rapid: is the Z dimension to transition from rapid to feed. Make sure that Z rapid is

set high enough to compensate for the amount of float in the floating tapping head.

Z End: the depth of the thread
PITCH - the distance from one thread to the next in inches or mm. It is equal to one

divided by the number of threads per inch. For exa mple, the pitch for a 1/4-20 screw is
1 ÷ 20 = .05 inches

RPM: spindle RPM
Tool #: is the tool number you assign

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual

74

Tap Size

4-40

AS

AS

AS

AS A

¼ - 20

AS

AS

AS

AS

AS

AS

A

1-8

A A

Tap Size

¼ - 20

AS

AS

AS

AS

AS

AS

A

½ -13

AS

AS

AS

AS

AS A

Tap Size

200

400

600

800

1000

8.14.1 DPMSX Tapping Spe ed Recommendations

A – aluminum only
AS – aluminum and steel

DPMSX2

40 100 200 300 500 750 1000

vs RPM

8-32 AS AS AS AS AS A

3/8 -16 AS AS AS AS AS AS A

½ -13 AS AS AS AS AS A

5/8 - 11 AS AS A A A

¾-10 AS AS A A

Interpolate speeds for tap sizes in between the ones noted in the table

DPMSX3 and DPMSX5

40 100 200 300 500 750 1000

vs RPM

4-40 AS AS AS AS A
8-32 AS AS AS AS AS A

3/8 -16 AS AS AS AS AS AS A

5/8 - 11 AS AS A A A

¾-10 AS AS A A

1-8 AS AS A

Interpolate speeds for tap sizes in between the ones noted in the table

8.14.2 FHM5 and FHM7 Tapping Speed Recommendations

FHM5 and FHM7

vs RPM

4-40 AS AS A
8-32 AS AS AS A

¼ - 20 AS AS AS AS A

3/8 -16 AS AS AS AS A

½ -13 AS AS AS A

5/8 - 11 AS AS A

¾-10 A A

Interpolate speeds for tap sizes in between the ones noted in the table

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual

75

8.14.3 Tapping Notes and Recommendations

• Harder materials will require slowe r speeds and tap size may also be limited. For

example, the TRAK Bed Mill may not be capable of tapping a 5/8-11 thread in
inconel.

• Softer materials than aluminum may be capable of higher speeds and you may be

able to go a little bigger in terms of tap sizes than what is listed in the table.

• Make sure your tap is not dull. Dull taps will re q uire more torque to cut and may not

cut threads to specification.

• Cutting oil will play a large role in determining the size of tap you can use in a given

material. In the tables above, cutting oil was used for the results shown for the DPM
SX2, SX3 and SX5. Coolant delivered by the optional spray coolant system was used
for the results shown for the FHM5 and FHM7.

• Before tapping make sure your holder has adequate float in the tension and

compression stroke. The holder should float up and down with minimal force applied
to the holder. Also make sure your holder does not stick in tension (holder pulls
down) or compression (holder pulls up). This will stop the tap from getting to the
correct position programmed and may also break your tap.

• Always set your Z rapid higher than the tension stroke of your holder. This will save

your tap if the holder does get stuck in the tension stroke between holes.

• Make sure your t ap is running tr ue in the holder.

• Most tapping problems are due to a dull tap or a holder that is not floating and is

stuck in a certain position.

• For Models FHM5 and FHM7, ¾ - 10 must be run at slow speeds and soft materials

only.

8.15 Engrave Event (Advanced Features Option)

The Engrave Event allows you to machine numbers, letters and special characters as part
of a part program. See Figure 8.14 below for the letters and special characters that are
available in the Engrave Event.

When programming with the Engrave Event, the ProtoTRAK will construct a box to
contain the text you define. This box is oriented along the X axis like the text in this
sentence, and you m ay program up to 40 characters per event (although you will only be
able to see 20 characters on the prompts screen). To machine text in a direction other
than the X axis, simply use multiple Engrave Events and place the lower left corner of the
box wherever you would like. The numbers and letters you program will always have a
standard orientation (like the letters on this page) – you cannot program tilted or
inverted letters with the Engrave Event. The letters are of the font shown in the figure
and all capitals.

Prompts for the Engrave Event:

First, define the lower left corner of the box that will contain your text:

X BEGIN: The X coordinate of where you wa nt your text to begin
Y BEGIN: The Y coordinate of where you want your text to begin
Z RAPID: The Z dimension where the Z rapid feed slows to Z program feed

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual

76

programmed text and will update as you enter each character

Z END: The Z dimensi on to the bottom of your text.
HEIGHT: The he ight of your text. Each character varies in width; the set height of the

character will change the width in order to keep the overall size of the character
proportional.

TEXT: The text to be milled. When you get to this prompt, the Alpha keys will
automatically pop up to allow you to e nter the text. Once you have finished entering
text, you must press End (F8) and then any of the SET keys to successfully ent er your
text into the event. The alpha keys will appear automatically if the text field is blank. If
you have already entered text but wish to make a change, you will see a blue question
mark appear on the lower left corner of the screen when you scroll to this field, press the
Help button and the alpha keys will appear.

RPM: is the spindle RPM for the event. INC SET will use the RPM of the previous event.
RPM programming is available only if the Programmable Electronic Head Option is active.

Z FEEDRATE: Is the feedrate from Z rapid to Z end
XYZ FEEDRATE: The feedrate of XYZ along the path of the text
Tool #: is the tool number you assign

.

Figure 8.14 The above figure shows the text and special characters available for the Engrave event.

Notice the field that is labeled “Text Length”. This field will display the total length of your

8.16 Finishing Teach Events

Teach events are e ither POSN, DRILL or MILL events that are originated in the DRO
Mode (see Section 6.7).

The Teach events that are started in the DRO Mode must be finished in the Program
Mode before running. Teach events are of these different types:

TEACH POSN - for two-axis operation, the Position and Drill event types are combined.
See Section 8.1 for a description of Position event prompts.

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual

77

TEACH DRILL- this may also be made into a bore event. See Section 8.2 for a
description of Drill event prompts.

TEACH MILL - a straight l ine that specifies the beginning and the end. When TEACH
MILL events are defined using the CONT MILL softkey, the prompts for information that
cannot change will be suppressed. See Section 8.4 for a description of Mill event
prompts.

When a Teach event is unfinished, the words NOT OK will appear next to the event type.
Once the prompts are completed, the words NOT OK and Teach will disappear. The
event will become a normal MILL, DRILL, or POSN event.

TRAK Bed Mill and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual

78

FIGURE 9.1 Once the profile header screen is finished, you choose between an A.G.E. Mill and an A.G.E.

Arc to define the shape

9.0 Program Mode

Part 3: The Auto Geometry Engine (A.G.E.) Programming

This entire section deals with the Auto Geometry Engine which is part of the Advanced
Features Option. If the Advanced Features Option is not active, the Auto Geometry
Engine is not available on your control. I f you sometimes need to program prints with
data missing, the Auto Geometry Engine alone is worth the price of the Advanced
Features Option. See Section 3.1.2 for more informati on about the Advanced Features
Option.

When you program an Irregular Pocket (Section 8.6.3) or an Irregular Profile (Section

8.8.3) the Auto Geometry Engine, or A.G.E. is automatically started.

The A.G.E. is powerful software that works behind the easy-to-use geometry
programming of the ProtoTRAK SMX CNC. It is treated in its own section because it
works differently than the other event types. Unlike other events, the A.G.E. allows you
to:

• Enter the data you know, and skip the prompts you don’t.

• Use different types of data (like angle s) that may be available from the print.

• Enter guesses for the X and Y ends and centers not a vailable on the print .

With the A.G.E., you can easily overcome limitations in the data the print provides
without having to spend time in laborious calculations.

9.1 Starting the A.G.E.

The A.G.E. is started automatically w hen you enter the Irregular Pocket or I rregular
Profile event. The first set of prompts you encounter will be the header information.
Once that information is entered, you will see the foll owing screen:

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual

79

FIGURE 9.2 A.G.E. Mill prompts. Enter what you know, skip or guess the ones you don’t

Where:

A.G.E. Mill: A straight line from one X Y point to another.
A.G.E. Arc: Any part of a circle.

End A.G.E.: Ends the A.G.E. programming for the Irregular Pocket or Irregular Profile.
Abort A.G.E.: Aborts all A.G.E. events. The data for all the events is lost.

9.2 A.G.E. Mill Prompts

Press the A.G.E. Mill key.

Prompts in A.G.E. Mill programming:
Tangent: this refers to the tangency of the mill to the previous event. See Section 9.11

for a discussion of tangency.

X END: is the X dimension to the end of the mill cut; incremental is X Begin
Y END: is the Y dimension to the end of the mill cut; incremental is Y Begin
CONRAD: is the dimension of a tangential radius to the next event
ANGLE END: is the angle measured counterclockwise from this mill event to the next.

Do not input if the next event is an arc

LENGTH: is the length of the mill from beginning to end
LINE ANGLE: is the angle of this mill line (mo ving from begin to end) measured

counterclockwise from the positive X axis (that is 3 o’clock)

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual

80

GUESS: This softkey will appear when the prompt is on X or Y dimensioned data. Press
the Guess key before you press INC SET or ABS SET to enter the data as a guess. See
Section 9.7 for using Guess and Section 9.8 for using the Graphics to enter a Guess.

9.3 A.G.E. Arc Prompts

Press the A.G.E. ARC key.
Prompts in A.G.E. Arc progra mming:
Tangent: this refers to the tangency of the mill to the previous event. See Section 9.11

for a discussion of tangency.

DIRECTION: is the clockwise (input 1), or counterclockwise (input 2) direction of the arc
X END: is the X dimension to the end of the arc cut; incremental is from X Begin
Y END: is the Y dimension to the end of the arc cut; incremental is from Y Begin
X CENTER: is the X dimension to the center of the arc; incremental is from X End
Y CENTER: is the Y dimension to the center of the arc; incremental is from Y End
CONRAD: is the dimension of a tangential radius to the next event
RADIUS: is the radius of the arc
CHORD LENGTH: is the straight line distance from the begin point to the end point
CHORD ANGLE: is the angle spanned by the arc

In addition to the normal Softkeys, this additional one will appear in A.G.E. Arc
programming:

GUESS: this softkey will appear when the prompt is on X or Y dimensi oned data. Press
the Guess key before you press INC SET or ABS SET to enter the data as a guess. See
Section 9.7

9.4 Skipping Over Prompts

In the A.G.E., events don't have to be fully defined before you can go to the next one.
You can skip the data you don’t know by using the DATA FWD softkey. After you press
the DATA FWD key at the last prompt, the event will move to the left side of the screen
and the Select Event screen will appear.

When skipping over prompts or editing, always use the DATA FWD or DATA BACK key.
Using INC SET or ABS SET will change the data.

If you want the eve nt back on the right side, use the BACK hard key.

9.5 The OK/NOT OK Flag

Each A.G.E. event has a flag that tells you if it has be en fully defined. Sometimes data
from later events is needed to define previous events. To the immediate right of the
event type, the words OK or NOT OK appear, depending on whether that particular event
is defined.

Once the OK flag appears for the event, you do not need to enter more information.
Skip past the rest of the prompts with the DATA FWD softkey.

If you leave the Program Mode and then return, pressing the GO TO END softkey will
take you automatically to the first NOT OK event.

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual

81

9.7 The X End dimension has been entered as a guess—note the letter G

9.6 Ending A.G.E.

Any time all the events are of an Irregular Profile are OK, the A.G.E. may be ended. If
you are programming an Irregular Pocket, there is an additional requirement that must
be satisfied before the A.G.E. may be ended: the X and Y end point of the last event
must be the same as the X and Y beginning point, so that the pocket is closed.
Otherwise, the ProtoTRAK SMX CNC cannot program the tool path to clear the pocket.

The Irregular Profile has no such restriction since profiles may be open or closed.
Once the A.G.E. is ended, the Irregular Pocket or Irregular Profile event is complete and

you may then choose from all the prog ramming canned cycles from the Select an Event
screen. To reopen the A.G.E. Profile or Pocket, simply use the BACK hard key or the
PAGE FWD or PAGE BACK softkeys to position on of the A.G.E. events on the right side of
the screen. You may edit or insert other events.

9.7 Guessing Data

Whenever you are missing X or Y Ends or Centers, you should generally enter a guess.
Guessed data is treated differently by the ProtoTRAK SMX CNC than regular data. Often,
the information you put into the system will allow it to ca lculat e a mathematically correct
line or arc that would satisfy the conditions of the hard data you entered. This line or arc
may yield more than one solution to particular point you are looking for. That is where
the Guess comes in: the A.G.E. uses the guess to choose from the mathematically
possible solutions. In most cases, your guesses do not have to be very precise. The
smaller the lines or arcs, the more precise the guess should be.

FIGURE

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual

82

Guesses should always be entered as absolute dimensions. Once entered, the guessed
data is green and there is a 'G' next to it. Guessed data will be labeled this way in all the
events that are flagged NOT OK. Once an event is OK, the guessed data will be replaced
by calculated data. If you wish to edit your guesses, placing it on the right side of the
screen will cause your original guessed data to reappear.

9.8 LOOK and Guess

Guessed data may be entered by pressing the number keys and then SET. However, you
may find it more convenient to use the LOOK graphics to enter guesses.

When the highlight is on the prompt for which you wish to enter a guess, press the
Guess key. The Data Input Line will say "Enter Guess for X END" (for example). At this
point, press the LOOK key.

Figure 9.8.1 When the Data Input Line says "Enter Guess" pressing LOOK gives you the ability
to use graphics to make your guesses.

On the screen shown in the figure above, the Data Input Line says "Enter Guess for X
BEG". Pressing LOOK at this point will take you to a special version of the LOOK
graphics. Using a m ouse or the cursor keys, you may move a point around the screen.
When you come to the place where your point is, use the Enter key.

The softkeys for this special version of the LOOK gra p hics:
ç è é ê: move the cursor around the screen.

ZOOM IN: makes the drawing larger.
ZOOM OUT: makes the drawing smaller.
ENTER END: when the cursor is at the point you want to use as a guess, use t his to

enter the end point of a line or an arc.
ENTER CENTER: use this to reg ister a guess for the center of an arc.

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual

83

9.8.2 When the events are calculated based on Guessed data, they are represented by a dotted line

You can enter a combination of guessed and non-guessed data. For example, if you
were to enter the dimension for X End without guessing, you would still be able to enter
the dimension of Y End using guess.

Your guess entries are loaded into the program when you exit the LOOK screen by
pressing BACK or by pressing LOOK again. The ProtoTRAK will use the last ENTER key
press and load that into the program.

When you use the graphics to guess dimensions on arcs, you may load in guesses for
both the X/Y End and the X/Y Center before leaving the LOOK screen.

When you have not first pressed the Guess key, pressing LOOK gives you the same
screen as in regular programming. Whether you enter the guesses as key presses or by
using the graphics , the drawing of the LOOK screen distinguishes between events that
are fully defined and those that rely on guessed data. OK events are represented by
solid lines. NOT OK events are represented by dashed lines.

FIGURE

9.9 Calculated Data

Prompts that are skipped or for which guesses are entered may be replaced by data
calculated by the ProtoTRAK SMX CNC. Ca lculated data is s ho wn in red in order to
distinguish it from the data that you entered. You cannot edit calculated data, but you
may edit your original input. By putting the event with the calculated data on the right
side of the screen, you may position the cursor to the prompt and re-input the data.

9.10 Arcs and Conrads

If the print is missing a lot of data, it may be desirable to program arcs as separate
events where possible. This gives the system more information to work with.

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual

84

9.11 Tangency

Tangency can occur between a mill and arc or an arc and arc. Specifically it means that
the two events share one and only one point. You would answer yes to the TANGENCY
prompt if the event you are programming is tangent to the previous event. The
information that events are tangent helps the Auto Geometry Engine calculate other
dimensions.

You can often tell by looking at the print if events are tangent: tangent intersections tend
to blend smoothly , without a sharp corner.

smooth, probably tangent sharp , not tangent

For the A.G.E., the tangent mill or ar c is assumed to continue in the same direction, and
not double back on the previous event:

like this not this

Southwestern Industries, Inc.

85

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual

10.2.1 The Search Edit softkey launches Spreadsheet Editing. View the entire program by the

variables you select

10.0 Edit Mode

Within Program Mode, you can recall and re-input specific data prompt by prompt. When
the Advanced Feature s Option is active the Edi t Mode contains powerful rout ines for
more extensive program changes.

The changes you make in the Edit Mode affect only the program in current memory. In
order to preserve the changes for future use, the program must be stored again under
the same name in the In/Out Mode.

10.1 Delete Events

To delete a group of events in the program, press Delete Events
The Data Input Line will prompt for the first event to be deleted. Input the event

number of the first event and press set. Next the Data Input Line will prompt for the last
event number to be deleted. Put in the last number and press Set.

The remaining events will be renumbered.

10.2 Spreadsheet Editing(Advanced Features Option)

FIGURE

Spreadsheet Editing allows you to view program inputs in a table and make global
changes to the program. This is particularly useful if you are working with a large
program and you need to make a change to many events.

When you press the SEARCH EDIT softkey, the screen will load a table that contains data
for every event. See Figure 10.2.1

86

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual

The first time the screen appears, the data is sorted by event number. Each row
represents the data for the event number show n i n the first column on the left. The
event number is always displayed in the first column, but the other data displayed on the
table can be changed.

Soft Keys in Search Edit:

PAGE FWD: pages forward through the table.
PAGE BACK: pages backwards through the table.

6534: highlights data for editing. Only data that is highlighted and appears in the
Data Input Line may be edited. Note: the EVT# (event number) and (event) TYPE may
not be edited in Search Edit so the highlighter wi ll not go there.

SORT: enables you to change the sort to any of the data displayed. See Section 1 0.2.2
CHANGE ALL: enables you to make global changes of data. See 10.2.3

10.2.1 Selecting Data to be Displayed on the Search Edit Table

In order to change the data selected in the table, press the HELP hard key. There will be
a listing of all the data types that may be edited in Search Edit. Press the RETURN soft
key and the table will be reloaded with the data that you selected.

FIGURE 10.2.2 Pressing Help while viewing the spreadsheet lets you change the program parameters

After you press the HELP hard key, the screen will display all the different parameters
that can be displayed on the spreadsheet. To either select or deselect any parameter,

87

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CN C Safety, P rogramming, Operating & Care Manual

simply highlight that parameter and press SET. When you are finished, pres s the Return
softkey and return to the spreadsheet.

10.2.2 Sorting Data

Data may be sorted by any of the data types displayed in the column head. Red letters
show which column is used for sorting the data.

To change the sort, press the SORT softkey, then select the type of data you want t o use
for sorting from the softkeys.

The table will be changed to sort the data in ascending order (the smallest value first, the
largest last).

10.2.3 Making Global Changes to Data

Sometimes it is useful to be able to change data in a program without having to go
through each event one at a time. For example, if you were to want to change the tool
number for every milling event, it may be a chore to go through each event in a long
program to make the changes on that event type.

In order to make global changes:

1. Sort the data in a way that groups together the things you want to change.

2. Highlight the data value that is highest on the table (nearest to the top) that you

want changed.

3. Press the CHANGE ALL softkey. All the inputs that are the same as the one you

highlighted and are listed together below the data you highlighted will then be
highlighted.

4. Enter the new value, then press set. All the highlighted data will be changed to the

value you just input.

Example:

From the screen shown in Figure 10.2.1, we will change the Z Feed for each of the mill
events in the program.

1. Sort by event type to get all the Mill events together.

2. Highlight the Z Feed in the first Mill event (Event # 8). See Figure 10.2.3

3. Press the CHANGE ALL softkey. All the Z Feeds in the Mill events are highlighted.

See Figure 10.2.4

4. Type in the new Z Feed value and press INC SET or ABS SET. See Figure 10.2.5

88

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual

FIGURE 10.2.3 After sorting by Event Type, the highlighter is placed on the Z feed of the first Mill Event

FIGURE 10.2.4 Pressing the Change All softkey highlights the Z feed for all the Mill events

In this example, the Z feed is changed from 5.0 to 7.0 for all the Mill Events.

89

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CN C Safety, P rogramming, Operating & Care Manual

10.2.5 Type the new Z Feed and then SET to change all the highlighted values from 5 to 7.

FIGURE

10.3 Erase Program

Use the ERASE PROG soft key to erase the program from the current memory. Erasing
the program from current memory will not affect any programs that are stored.

If you have made changes to the program and wish to save this modified program, you
will need to store it. See Section 13.4

10.4 Clipboard (Advanced Features Option)

The Clipboard feature is a way to copy events in one program in order to put them into a
different program. It is a two-part process that takes place in two different Modes. First,
in the Edit Mode, the desired events are copied, or placed on the Clipboard, from the
source program. Then the events are inserted into the destination program in the
Program Mode.

When you press the Clipboard key from the Edit Mode, you start the process that copies
the events that you want to put into a different program than the one in current memory.

Before you do that, you should write a program or open the program file that has the
events you want to copy. This is called the source program.

Inspect the events you wa nt to copy. Make sure that the dimensioned data uses
Absolute references in the first event to be copied and in all events where it will be
important. Incremental references may be used, but keep in mind where the
Incremental reference will be made from. See the section on Incremental Reference
Position in this manual.

90

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual

i01142

In addition, you may want to modify this program in order to get all the events you want
together. For example, if you want to copy events 2-5 and 7-12, you may want to
modify the program to delete events 1 and 6 first. That way, you can copy the all the
events as they are now numbered from 1 to 10. Remember that you can modify this
program just for this purpose and it will not affect the original program unless you save it
with the modifications in the Program In/Out Mode.

When the source program is ready, press the CLIPBOARD softkey. A message will
appear that says "Copy Events Onto Clipboard" and the Data Input Line will read "From
Event". Enter the numbe r of the first event that you want copied and press SET.

The Data Input Line will re ad "To Event". Enter the number of the last event you want
copied and press SET.

The group of events that you have specified is now on the clipboard and will remain
there until you replace it with something else by go ing through the same procedure.
When power is turned off to the CNC the clipboard information will also be lost.

The events on the clipboard are inserted into a program in the Program Mode. See
Section 8.11.

10.5 G-Code Editor (Advanced Features Option)

The G-Code Editor allows the edit of G-Code programs that are opened as .GCD files.
Once edited, the program may be re-saved as .GCD files. ProtoTRAK Geometry-style
programs may not be saved as .GCD files.

Figure 10.5.1 Use the G-Code E ditor to modify G-Code programs.

91

Southwestern Industries, Inc.

TRAK Bed Mill and ProtoTRAK SMX CN C Safety, P rogramming, Operating & Care Manual

Figure 10.5.2 The find and replace routine.

You must connect a mouse and keyboard in order to use th e G-Code Editor.
When you enter the G-Code Editor, the G-Code program is displayed starting at the first

Block Number. Use the scroll bar to move up and down through the program. Use the
mouse and keyboard to edit like you would an MS Notepad™ file.

Search allows you to launch a simple find-and-replace routine to aid in editing large G­Code files.

Click in the Find What box and enter the item you want to find. Click on the Find Next
box and the G-Code Editor will locate the next occurrence of that item. Successive clicks
on Find Next will continue to search through the program. Use Match Whole Word to
limit the search to the entire word. For examp l e, if you want to find G2, but not G20 or
G22, select Match Whole Word Only.

Instead of typing the item into the Find What box, you may simply highlight an item on
the G-Code Editor screen. That item will be entered into the Find What box for you.

To make changes to Find What items, type what you w ant to have into the Replace With
box. You can replace items one at a time by clicking first the Find Next box then the
Replace With box for as many changes as you want to make. You can replace every item
in the program with a single click of the Replace All box.

Return closes the G-Code Editor and returns the screen to the Edit Mode.
Note: If you use the USB Thumb Drive to store a G-code (.gcd) program file, you must

leave the Thumb Drive plugged into the USB port the entire time the program is in
current memory. If you unplug the thumb drive with the program still in current
memory, the ProtoTRAK will display an error message.

92

Southwestern Industries, Inc.

TRAK Bed Mills and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual

i0114

11.0 The Set-Up mode

FIGURE 11.1 The Tool Table

11.0 Set Up Mode

The Set Up Mode contains the tool library, the tool path and verify graphics and the machine's reference
positions. Enter the Set-Up Mode by pressing the SET-UP soft key at the Select Mode screen.

11.1 The Tool Table

From the screen above, press the TOOL TABLE softkey.

FIGURE

93

TRAK Bed Mills and ProtoTRAK SMX C NC Safety, P rogramming, Operating & Care Manual

11.1.1 The Tool Table Screen

When you first enter the tool table by pressing the TOOL TABLE soft key, you will see the
screen shown in Figure 11.1.

Tool #: the number of the tool from 1 to 99. Tool numbers shown in red are active for the
program in current memory.

Diameter: the diameter of the tool.
Z Offset: the difference between the Z position of the tool and the Z position of the

reference. The Z offset is always relative to a reference point. Before the reference point is
set, the highlight will not go into the Z Offset column because setting a Z offset before the Z
reference is set has no meaning.

Z modifier: a value you enter to make adjustments for the tool depth. See 11.1.7 below.
Tool Type: allows you to select the type of tool from a list. Input the number that

corresponds to the desired name (eg 1 = Drill) and press SET. The tool name will be in the
prompt at the begi nni ng of the program Run.

Ref: the reference position for the Z offset. Before the reference position is set (and the
Ref row reads "NOT SET") the highlight will not go into the Z Offset column. Once it set,
the highlight will not go into the Ref row, that is, you will not be able to highlight and reset
your reference once it says "SET".

The soft keys in the tool table:

DATA DOWN, DATA UP, DATA LEFT, DATA RIGHT: move the highlight around the table.
ERASE TABLE: clears all tool information so you can start over. See 11.1.4 below.
JOG: puts the ProtoTRAK SMX CNC into the DRO jog operation (see Section 6.3).
RETURN: reverts to the SET UP mode screen.

The electronic handwheels are active, including the fine/coarse selection, while you are in
the tool table.

11.1.2 The Logic of the Tool Table

The tool table is organized to do the following:

• Make it easy to set up tools.

• Make it easy to replace a tool or add a tool.

• Retain tool information in memory to reduce set-up.

You assign tool numbers as you write a program. These tool numbers may be from 1 to 99.
Before machining, the diameters and Z offset of each of the tools in the program must be
defined so that the ProtoTRAK SMX CNC can calculate the tool path. Tools that are used in
the program that is in current memory are called active tools and their numbers are in red in
the tool table.

When you save a program, all the tool information for active tools is saved with it. When
the program is opened, the tool information is put into the tool table. This information will
replace any information that alre ady is in the tool table for the same tool numbers.

In addition to information about the tools used in a program, you may load in information
for tools to be used in 2-axis CNC or in the DRO mode for machining manually. When you
tell the ProtoTRAK SMX CNC which tool you are using, it will adjust the Z DRO dimensions
accordingly so you don’t have to touch off and reset after a to ol change.

The idea of retaining tool information in memory in order to reduce the amount of set-up
needed requires that care be taken to avoid mistakes. Milling work usually requires a lot of

Southwestern Industries, Inc.

94

Southwestern Industries, Inc.

TRAK Bed Mills and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual

tools, many of which are not preset into fixed tool holders. That means tool information
that is not very recent is probably no good.

Think of the information in the tool table this way: if you clearly remember setting the tools
and entering the diameters very recently, then use the tool table in DRO and CNC run. If you
can't remember setting the tools clearly, erase the table and start over – it only takes a
moment.

This may cause some confusion because the normal sequence for running a two-axis
program is to load in a tool, touch it off and set zero, then press GO. The ProtoTRAK SMX
CNC will apply the tool offset after the GO press, making the Z dimension meaningless.

You have two choices:

1. Use the tool table, setting the reference and absolute dimension for one of them per the

instructions above. This will save you from having to touch off tools every time they are
changed in program Run.

2. Don’t use the tool table. Erase the entire tool data so that the ProtoTRAK SMX CNC will

not try to apply offsets.

11.1.3 Initial Tool Set-Up

This procedure is used for setting up tools when the tool table is clear.

1. When you enter this screen for the first time, the words "NOT SET" appear directly under the

Z OFFSET column in the REF row. The Data Input Line reads "TOUCHOFF REFERENCE
POINT". This is prompting you to establish a reference for the rest of your tools.

2. To establish a reference, put a cutting tool or some other reference setting tool into

the spindle and touch the to ol to a surface. We recommend that you use something
besides a tool that you intend to use machining the job. Ideally, you will have a
reference tool that you keep handy for setting up your tools every time. That way, a
reference point can be easily re-established later.

3. We also recommend that you use the top of the vise or table as your reference

surface because it is constant and never changes.

4. With t he highlight on the screen on the words "NOT SET" and the tool touching some

reference point, press SET.

NOTE: If you do use a tool as your reference tool and it breaks, you must retouch off all tools.

5. The words will change from "NOT SET" to "SET" and the highlight will shift to the

DIAMETER column of Tool # 1. (Note that you may not be interested in setting up
Tool #1 if it is not one of the active tools of the program. If this is the case, use the
DATA softkeys to move to a tool you are interested in.)

6. Input the diameter for the tool and press SET.

7. The highlig ht will move to the Z OFFSET column. Put this tool in the spindle and

touch it to the same surface as you used to touch the reference tool in Step 2 above.

8. Press set.

9. The highlight moves to the Z Modifier column. Input and set a Z modifier if you wish

(see below) or simply press SET to input no modifier.

10. The highlight moves to Tool Type and a green window appears with your choices.

Input 1 to 9 corresponding to your choice and then SET. This moves you to the
Diameter input for your next tool.

95

TRAK Bed Mills and ProtoTRAK SMX C NC Safety, P rogramming, Operating & Care Manual

11. Repeat steps 5 to 8 for each of the tools you want to set up. Remember to t ouch the

same surface you used to set the reference tool.

Once the reference position is set, you will not be able to move the highlight back to the
word "SET".

Note: You must set an absolute zero reference in the DRO Mode before machining the part. You may
use any tool that you have set up with the above procedure to set your reference and the ProtoTRAK
will automatically compen sate for the difference in length for the rest of the tools.

11.1.4 Starting Over: Erasing Tool Information

There will be times when you don't completely trust the information that is in the tool table.
For example, perhaps you have loaded in a program that you wrote a month ago and you
recall that one of the tools you used was held in a chuck. In that case, you probably want
to erase the table and start over.

In order to do this, simply press the ERASE TABLE softkey and answer yes to the prompt.
All the data in the tool table will be erased including the reference. The numbers of the
tools used in any program in current memory will still be red.

11.1.5 Adding a Tool

When the reference is SET and the original touch-off surface is still available, you can add a
tool very easily:

1. First make the tool number active by using it in the program in current memory.

2. Put the new tool in the spindle.

3. Go to the Set-Up Mode, tool table

4. Enter the diameter.

5. Touch the new tool to the same surface as the reference.

6. Press SET.

If the surface is not available, it will be necessary to establish a new reference before adding
the new tool. See Section 11.1.8 below. Once the reference is reset, use the procedure
above on the new surface used to set the reference.

11.1.6 Replacing a Tool

If you need to replace a tool that was not used as the reference, simply do the following:

1. Put the replacement tool in the spindle.

2. Put the highlight in the correct row for the tool number.

3. Reenter the diameter if different.

4. Touch the tool to the same surface that was used to touch off the reference.

5. With the highlight in the Z OFFSET column for the correct tool number, press SET.

If you need to replace a tool that was used as a reference, we recommend that you press
the ERASE TABLE softkey and start all over again. (Not to nag, but that is why it is a good
idea to have a separate reference setting tool and use a constant reference surface. If you
work with programs that use a lot of tools, this practice can really save time.)

Southwestern Industries, Inc.