Trak Lathe Guide

Machine guide for the Trak lathe

Table of Contents

Overview

The Trak TRL 1540V is intended for medium sized CNC work. With a few minor exceptions, manual machining should not be done on this machine. The machine’s X & Z limits are 5” x 40” (127mm x 1016mm). The machine has a spindle speed range of 150 to 4000 RPM with a maximum feed rate of 50 IPM (1270 mm/m) in the X & Z axis.

Trak Lathe

Control Panel

Control Panel

The control panel is the primary control interface for the machine.

Remote Stop/Go Switch

Remote

The remote stop/go switch is a hand-held remote equivalent to the STOP/GO button on the control panel.

Apron

Carriage

The apron is where the X & Z handwheels are located, along with the jog stick. You should familarize yourself with these controls and how they function.

Chuck

Chuck

The chuck is used to hold your part. It has the capability to hold stock up 9”. If your stock exceeds 4”, you will need to reverse the jaws. Speak with one of the professional staff before reversing the jaws.

[warning]Do not exceed 2200 RPMs, 1000 RPMs if the jaws are reversed.

The chuck is rated for a maximum 2200 RPMs. If the jaws are reversed, the maximum speed is 1000 RPMs. Exceeding the maximum RPM could result in damage to the chuck, machine, and potentially yourself.

Jaws Reversed

Jaws reversed

Collet Closer

Collet closer

The lathe can use 5C collets when the chuck is replaced with a collet closer. These can run at speeds up to 4000 RPMs, but consult with professional staff before doing so.

Tool Post

Tool Post

Tailstock

Tailstock

The tailstock is used for drilling, when a drill chuck is installed, or supporting the material, by using a live center.

Startup procedures

[warning]Part of the startup procedure below will cause the machine to move automatically. If for any reason the machine starts to do something unintended hit the large red emergency stop button on the control panel.

Turn on main power switch, located in the back left side of the lathe.

Main power switch

Flip toggle switch on lathe controller to the on position (up).

Toggle switch

Once the controller is booted up,(approximately 90 secs), the Southwest Industries logo and name of software (ProtoTRAK VL) will appear on the screen with an orange colored background.

When prompted press the Check Systems soft key button.

Check systems button

Make sure the carriage is in a safe position away from the chuck and the tailstock (Approximately 2 to 3 inches).

Use the hand wheels to move carriage and cross slide in a safe position if need be. Make sure there are no tools in the tool post or tailstock.

Press the soft key labeled GO. Machine will home itself by moving slightly in both X and Z axis.

Go soft key

Control panel will ask for the maximum spindle rpm. Max spindle speed for the chuck is 2200 RPM or 1000 RPM if the jaws are reversed.

The max spindle speed is 4000 RPM when using the collet closer.

Use the keyboard on the control panel to type in max rpm and then press ABS SET to enter.

ABS

The max rpm can be modified at any time by pressing MODE, SETUP, MAX RPM, then entering a new rpm number then press ABS to enter. Press MODE to get back to main screen.

Activate the lubrication system by pressing MODE, SETUP, SERV CODES, E, CODE 300.

Servo code

You will hear the lubrication pump activate and the message Switch on lubrication pump wait will appear on the screen.

Wait until pump shuts off (approx. 15 secs).

The machine is now ready for use.

The tailstock is used for drilling,with a drill chuck,and for supporting the material, with a live center.

Placing stock in the Chuck

Place stock in chuck, leaving enough sticking out so the tool will not hit the chuck in the Z axis.

Stock

Note: If stock hangs out of the chuck more than 1 ½ times the diameter, you will need to use the live center located in the 5th drawer down in the red tool box.

Use chuck key to tighten jaws starting with the master marked with a 0. Rotate chuck and tighten the other 2 keys.

Measure diameter of the stock and write it down on your drawing. You will type in this measurement later. (See Setting Tools on the Tool setup page).

Tool Setup

Squaring the tool post

Loosen the nut on the top of the tool post using the provided box end wrench (do not use an adjustable wrench).

Press MODE on the controller, then press DRO to activate the jog stick and hand wheels.

Use the jog stick to position the tool post so it is centered in front of the tailstock.

Unlock the tailstock and bring it close to the carriage.

Unlock the tailstock ram, then extend the tailstock ram until its face comes into contact with the side of the tool post.

The tool post t-nut must be flush with the front side of the tool post mounting fixture (closest to the chuck/spindle).

Align the tool post square against the face of the tailstock.

Tighten the nut on the top of the tool post while keeping tool post square to tailstock face.

Now that tool post is square return tailstock to the end of the ways.

Preparing Tools

The tooling for the Trak lathe is located in the red tool cart next to the machine.

Ask shop staff to unlock the tool box and assist you in selecting and setting up your tools.

Identify the cutting tools and tool holders you will need to complete the part.

At minimum you will need a live center to center your tool(s) and presumably a right hand turning tool to turn and face your stock.

Centering Tools

Extend ram from tailstock and insert a live center into the tailstock.

Insert a tool into the tool post so that the tip of the tool faces the tailstock.

Press MODE on the controller, then “DRO” to move the hand wheels.

Adjust the carriage and tailstock so that the tip of the tool can be easily aligned with the tip of the live center.

Loosen the locking nut on the tool holder, then use the height adjustment screw to align the tip of the tool to the tip of the live center.

Once aligned, tighten the locking nut on the tool holder finger tight.

Repeat this process to center each tool.

Deleting existing tool table

Press MODE, SET UP and TOOL TABLE. Press the ERASE TABLE soft key, YES, then RETURN to remove all tools listed.

Erase tool table

Note: This will erase an existing tool table before creating a new one.

Setting tools

Press Mode, Setup, Tool setup .

Press Tool number. If this is the 1st tool being used in your program, type in 1 and ABS.

Press New for new entry or Edit to edit existing tool.

Set new/ edit

Note: Selecting Edit will allow you to edit a tool already in the Tool Table you just created.

Select New and ABS. This will bring you to the Tool list page which will look like this. 

Tool list

The numbers on the left of the screen correspond with tool type on the right side of the screen. 

If you were using a Right hand turn/face tool you would type the #1 and ABS. 

Another example would be if you need an OD Groove tool, you would select #10 as the type and ABS.

WARNING: Do not use #4 Back Bore, #5 Drill, #9 Button Tool and #12 Tapping Tool.

This brings you to the Tool setup page

Tool setup page

Turn spindle on by pressing Spindle FWD button on controller.

Using the jog stick or the hand wheels, on the carriage, bring tool close to OD of stock.

Press the F/C button on controller. This will change the feed from coarse(C) to fine (F). Must be in Fine to touch off OD. 

Note: If feed is left on Coarse, you may gouge tool into part giving you an inaccurate reading.

Once tool slightly touches OD, press X, then 0 and ABS. Press data back button to return to X axis. Move X handwheel to -.02. Now move Z handwheel to take a light cut off the OD far enough to measure the OD. Bring Z axis straight back away from the face of the part. Do not move the X axis. Shut off the spindle. Measure the OD with caliper or micrometer. Enter dimension in the box and press ABS. This gives a known value in the X axis from center of the chuck.

Move same tool to face of the part and lightly touch off the face.

If your program has a facing operation using the same tool, then you can zero the Z axis by pressing Z on the controller and 0 ABS.

If you don’t have a facing operation in your program, you may want to take small face cut 1st using the hand wheel and then zero the z axis after the face cut.

If you are running a CAM program, enter a 0 for the nose radius.

NOTE: If you enter a number for nose radius, the size of your part will be off by the amount entered when running a CAM program!

X modifier: is a value you input to adjust the diameter of your part. A positive # adds to the diameter that much larger.

Z modifier: is a value you input to adjust the depth in the Z axis. A positive # stop it that much away from the chuck.

X and Z MODIFIERS are for adjusting the final dimensions if needed. Only use these once you have consulted with an Instrument Maker. These adjustments can be made in the Tool Setup Page or Tool Table.

NOTE: Please use the Tool Table to make these adjustments. It's easier to navigate to.

Repeat these steps for each tool in your program.

Note:Be aware that each tool from the tool list page will have a different point of orientation on the tool setup page. The tool setup page will show where the tool should be referenced in both the X and Z axis. See photo above.

Basic Machine Operation

Note: Need to be in DRO screen to operate manual functions on the lathe.

Moving the Carriage

Press Mode, then DRO. This activates both X and Z axis jog handle and hand wheels.

Carriage

Now you can use the jog handle (or hand wheels) to position both carriage and cross slide to any position within reason. 

The hand wheels are controlled by servo motors, which means you will not feel any resistance when turning the hand wheels.

You must exercise extreme caution when moving the machine manually.

The hand wheels can be set to move at a Fine or Coarse rate of speed by pressing the F/C button located just above the upper left side of number pad on the control panel. F for fine / C for coarse. (Place Photo)

NOTE: It is a good idea at this point to practice moving the axes with the jog stick and hand wheels located on the apron.

Starting the Spindle

Press MODE, DRO, and SPIN SPEED.

If you would like to set spindle speed in RPM, type in the desired number, then INC SET.

If you would like the spindle speed in SFM, type in desired number them ABS SET. 

Inset

Select the direction the spindle will move by pressing FWD or REV.

Forward will rotate the spindle counterclockwise when facing the spindle.

This is the direction you will use to do the majority of your machining.

To turn off spindle by pressing the OFF button, between FWD and REV.

Forward

Feed Rate and Spindle Speed Override

The run feed rate may be changed at any time by pressing the FEED UP or DOWN arrow keys.

Each press increases or reduces the programmed feedrate, as well as rapid by 10%.

The spindle speed may be changed at any time by pressing the SPEED UP or DOWN arrow keys.

Each press increases or decreases the programmed speed by 5%. 

Feed/Speed override

Zeroing and presetting Axes

Refer to Setting Tools on the Tool Setup page. Tool(s) will be set using this process at all times.

Even if it is a simple program with 1 tool.

The tool number and the X, Z reference numbers will transpose from the Tool Setup Page to the DRO, given the correct tool number is displayed on the DRO page.

Coolant

Note: Check with shop staff before using coolant.

Coolant

Coolant can be turned on by pressing the ACCESSORY button once.

Turn it off by pressing it again.

If you would like the coolant to turn on while the program is running, press and hold the button for 3 seconds.

The coolant will turn on when the spindle turns on.

If you are running a CAM program, you will need manually press the accessory button.

Do One Events

The purpose of DO ONE events are to allow you to make simple chamfer, taper, radius, and fillet moves, one at a time, within the DRO mode and without the need to create an entire program.

Do one

The tool must be in the proper position before you select DO ONE.

It will move in the desired Taper, Radius or Fillet at the position it is currently located.

You can change the tool position only while you are in the DRO mode.

Taper

Press DO ONE. Select TAPER.

Taper

When you select TAPER, you will be prompted to enter a taper angle. The system defaults to a 45 degree taper.

If this is the angle you wish, press ABS SET.

You may specify any other angle by inputting the number and pressing ABS SET.

A positive number is set to do an outside taper, while a negative number does an internal taper.

You can now start the spindle and turn either of the hand wheels and the tool will move in the desired angle. (The spindle could be FWD or REV, depending on the part and setup).

Note: You may need to take several passes if it is a large Taper, stepping closer to the finish position instead of taking it all in one pass.

Radius

Press DO ONE and select RADIUS.

Radius

You will need to input a radius value and press ABS.

A positive number is designed to place a radius on the outside edge, by moving the carriage in the X positive direction.

A negative number will place the radius on the inside edge of a hole, by moving the carriage in the X negative direction.

You can now start the spindle and turn either of the hand wheels and the tool will move in the desired radius. (The spindle could be FWD or REV, depending on the part and setup).

Note: You may need to take several passes if it is a large RADIUS, stepping closer to the finish position instead of taking it all in one pass.

Fillet

Fillet

Press DO ONE and select Fillet. You will need to input a radius value and press ABS.

A positive number is designed to place a radius on the outside edge, by moving the carriage in the X positive direction.

A negative number will place the radius on the inside edge of a hole, by moving the carriage in the X negative direction.

You can now start the spindle and turn either of the hand wheels and the tool will move in the desired Fillet radius. (The spindle could be FWD or REV, depending on the part and setup).

Note: You may need to take several passes if it is a large Fillet, stepping closer to the finish position instead of taking it all in one pass.

GO TO

Go To is a function in the DRO mode that allows you to enter a dimension in the X and/or Z at which you want the machine to stop at that dimension.

Go to

The carriage will stop at the Z dimension you entered and the cross slide will stop at the X dimension you entered.

Note: Before turning on spindle and cutting in the Go To Mode, move tool safely away from the stock and make sure carriage and cross slide will stop at the X and/or Z dimensions you set.

Press GO TO, and enter the value for the X or Z axis, or a combination of both.

Press INC SET or ABS SET. Using the appropriate hand wheel, motion will stop at the entered dimension even if you continue to move the hand wheel.

POWER FEED

Do not use!

Conversational Programming

Program Events

To begin, press MODE, PROG, and then enter a program number and press ABS SET.

Ignore Event Comments, because the keyboard is not connected to the controller.

Now press GO TO BEGIN to start at the beginning of the program.

By using either the GO TO END or GO TO # buttons, you can jump to the end or the line number of an existing program.

If there is a program in the controller, delete the program by pressing MODE, EDIT, ERASE PROG, YES.

Cycle Events

The cycle event is not a single event, but rather a group of Turn and Arc events.

It allows you to program complex shapes (including the shape of the starting material) that require several roughing passes without the need to program each tool motion step.

Parts are programmed by first defining the profile of your finished part, then defining the profile of the stock.

Prompts for the initial Cycle screen:

X BEGIN: the X dimension to the beginning of the cycle.

Z BEGIN: the Z dimension to the beginning of the cycle.

DEPTH OF PASS: is a specified amount of material to be removed on each pass. When the highlight is on this prompt, the blue ? will be displayed on the screen next to the HELP key. If you press the HELP key, you will be given the choice of changing this prompt to # of PASSES. # of PASSES: is the number of equal depth cuts used to rough the part.

APPROACH: is to select if the roughing is to be done along X with facing passes (input 0, SET), or along Z with turning passes (input 1, SET).

RPM/SURFACE SPEED: is the spindle speed. Enter data and press INC SET for RPM or ABS SET for SFM.

FEED PER MIN OR REV: is the roughing feedrate. Enter data (0.1 - 99.9 IPM/2.5 - 2500 MMPM) and press INC SET for inch per minute (IPM) feed or enter data (0.001 - 0.099 IPR/0.025 - 2.5 MMPR) and press ABS SET for inch per revolution(IPR) feed.

TOOL #: is the number you assign to the roughing tool in the tool table.

FIN CUT: is the depth of the final finish cut made with the finishing tool.

Note: If you want a finish cut in the Z axis. Press Help next to the ? , it will ask if you would like to add a Z finish cut. Press YES soft key. A line will be added underneath FIN CUT that says Z FIN CUT. Type in the amount of stock to finish in the Z ABS Set. 

Help

FIN RPM/SURF SPEED: is the spindle speed. Enter data and press INC SET for RPM or ABS SET for SFM or SMM.

FIN FEED MIN/REV: is the finishing pass feedrate. Enter data (0.1 - 250 IPM/2.5 - 6350 MMPM) and press INC SET for inch per minute feed or enter data (0.001 - 0.250 IPR/0.025 – 6.35 MMPR) and press ABS SET for inch per revolution feed.

FIN TOOL #: is the number you assign to the finishing tool in the tool table.

When the screen is complete, the ProtoTRAK VL CNC will prompt you to input a series of TURN, ARC and POSITION events to describe the part and the original material.

The first screen will have the soft keys:

CYCLE TURN

CYCLE ARC

CYCLE POSN

END CYCLE

ABORT CYCLE

You will define the finished part with CYCLE TURN and CYCLE ARC events.

Follow this by defining the shape of the original material with CYCLE POSITION events.

When the last CYCLE POSITION event is defined it must end where the first cycle event began.

Press the END CYCLE soft key to end the cycle event.

If the last CYCLE POSITION event does not end at the beginning of the first cycle event, the system will prompt you that the cycle is not “Closed” and ask for a YES or NO response.

If YES is selected, the system will automatically enter a closing CYCLE POSITION event.

If NO is selected, you may enter your own closing CYCLE POSITION event(s).

LOOK may be used to view the completed cycle event without each tool pass displayed.

Press MODE, SETUP, TOOL PATH to display all tool passes.

Turn Events

Note: This event turns to size with 1 cut. If there’s a lot of stock to remove, use Cycle events.

This event allows you to turn in a straight line from any one X, Z point to another, including an inside or outside taper.

This event should be used for facing since this is also a straight line move from one X, Z point to another.

The event may be programmed with a CHAMFER or CONRAD if it is connective with the next event.

Note: The event tool motion will be to rapid to the X BEGIN, Z BEGIN position, then feed to X END, Z END with consideration for CHAMFER or CONRAD if one is programmed.

Prompts for the TURN event:

X BEGIN: is the X dimension to the beginning of the cut (diameter).

Z BEGIN: is the Z dimension to the beginning of the cut.

X END: is the X dimension to the end of the cut; incremental is from X

BEGIN.

Z END: is the Z dimension to the end of the cut; incremental is from Z BEGIN.

CHAMFER/CONRAD: is the dimension of a chamfer to tangential radius to the next event. Use ABS SET for chamfer, or INC SET for conrad.

TOOL OFFSET: is the selection of the tool offset to right (input 1, face or inside diameters), offset to left (input 2, outside diameters), or tool center–no offset (input 0) relative to the programmed edge and direction of tool cutter movement.

RPM/SURFACE SPEED: is the spindle speed. Enter the data and press INC SET for RPM or ABS SET for SFM or SMM.

FEED PER MIN/FEED PER REV: is the turning feed rate. Enter data (0.1 - 99.9 ipm/2.5 - 2500 mmpm) and press INC SET for inch per minute feed or enter data (0.001 - 0.099 ipr/0.025 - 2.5 mmpr) and press ABS SET for inch per revolution feed.

TOOL #: is the tool number you assign in the Tool Table, from 1-99.

Arc Events

This cuts an arc to size in 1 cut! If you have a lot of material left, use CYCLE.

This event allows you to turn with circular contouring any arc.

The event motion will be to rapid to the X BEGIN, Z BEGIN position, then feed to X END, Z END in a circular path.

Prompts for the Arc event:

X BEGIN: is the X dimension to the beginning of the arc cut (diameter).

Z BEGIN: is the Z dimension to the beginning of the arc cut.

X END: is the X dimension to the end of the arc cut, incremental is from X BEGIN.

Z END: is the Z dimension to the end of the arc cut, incremental is from Z BEGIN.

RADIUS: is the radius of the arc (not measured in diameter).

CHAMFER/CONRAD: is the dimension of a chamfer or tangential radius to the next event. Use ABS SET for a chamfer, or INC SET for conrad.

DIRECTION: is the clockwise (input 1), or counterclockwise (input 2) direction of the arc looking down from the top.

TOOL OFFSET: is the selection of the tool offset to right (input 1, face or inside diameters), offset to left (input 2, outside diameters), or tool center–no offset (input 0) relative to the programmed edge and direction of tool cutter movement.

RPM/SURFACE SPEED: is the spindle speed. Enter the data and press INC SET for RPM or ABS SET for SFM or SMM.

FEED PER MIN/FEED PER REV: is the Z boring feedrate. Enter data (0.1 - 99.9 ipm/2.5 - 2500 mmpm) and press INC SET for inch per minute feed or enter data (0.001 - 0.099 ipr/0.025 - 2.5 mmpr) and press ABS SET for inch per revolution feed.

TOOL#: is the tool number you assign in the Tool Table from 1-99.

Position Events

This event positions the tool at a specific position.

Note: The positioning is always at rapid speed and in the most direct path possible from the previous location.

Position is most often used to move the tool away from the part so that when it rapids to a next non-connective event or home, it will not crash into the work piece.

To program a Position event press POSN.

Prompts for the Position event:

X: is the X dimension (diameter)

Z: is the Z dimension (length)

RPM/SURFACE SPEED: is the spindle speed. Enter the data and press INC SET for RPM or ABS SET for SFM (surface feet per minute).

CONTINUE: asks you if you want to continue to the next event (press 1, SET), or pause after the tool is at position (press 0, SET).

TOOL#: is the tool number you assign in the Tool Table from 1-99.

Groove Events

The Groove event allows you to program an ID or OD groove along the length of your part.

It requires the use of a grooving tool with a defined width.

Prompts for the GROOVE event:

X BEGIN: The diameter at the beginning of the groove.

Z1: The Z dimension at the beginning of the groove.

Z2: The Z dimensions to the bottom of the groove.

X END: The X diameter at the bottom of the groove.

Z3: The Z dimension for the length of the bottom of the groove.

Z4: The Z dimension at the end of the groove.

CHAMFER/CONRAD TOP: allows a lead in chamfer or tangential radius at the beginning of the groove.

Use ABS SET for a chamfer, or INC SET for a conrad. Chamfer or conrad top will apply to X BEGIN, Z1, and Z4.

Chamfers or conrads at the top of your groove are calculated by assuming the intersecting line to the groove is parallel to the center line of the part.

CHAMFER/CONRAD BOTTOM: allows a chamfer or tangential radius at the bottom of the groove.

Use ABS SET for a chamfer, or INC SET for a conrad. Chamfer or conrad will apply to X END, Z2 and Z3.

RPM/SURFACE SPEED: is the spindle speed. Enter the data and press INC SET for RPM or ABS SET for SFM or SMM.

FEED PER MIN/FEED PER REV: is the roughing feed rate. Enter data (0.1 - 99.9 ipm/2.5 - 2500 mmpm) and press INC SET for inch per minute feed or enter data (0.001 - 0.099 ipr/0.025 - 2.5 mmpr) and press ABS SET for inch per revolution feed.

FIN CUT: is the depth of the final finish cut made.

The default setting for this event is to do the finish cut along the profile in one continuous move.

When the highlight is on this prompt, the blue ? will be displayed on the screen next to the HELP key.

If you press the HELP key, you will be given the choice of changing the finish cut setting to do PLUNGE AND SIDE CUTS ONLY.

The tool will plunge down each side of the groove and cut to the center of the groove. The second plunge and side cut will overlap the previous one.

FIN RPM/SURFACE SPEED: is the spindle speed. Enter the data and press INC SET for RPM or ABS SET for SFM or SMM.

FEED PER MIN/FEED PER REV: is the turning feed rate. Enter data (0.1 - 99.9 ipm/2.5 - 2500 mmpm) and press INC SET for inch per minute feed or enter data (0.001 - 0.099 ipr/0.025 - 2.5 mmpr) and press ABS SET for inch per revolution feed.

TOOL#: is the tool number you assign in the Tool Table from 1-99.

The tool path of the groove event starts in the center of the programmed groove and works its way to each side, followed by the finished cut (if programmed).

All roughing is done along the X axis except where the walls are angled.

For the angled sections, the tool will plunge along the X axis and then follow the contour of the angled wall.

Thread Event

Please see Professional staff before attempting!

This event allows you to machine standard or custom I.D. or O.D. threads.

They may be straight or tapered, and may be one through ten multiple leads.

The event motion will be to rapid to the X BEGIN, Z BEGIN position, then feed to a depth equal to the total thread depth adjusted for the number of passes, feed to X END, Z END, rapid away from the thread, return to X BEGIN, Z BEGIN and repeat for the total number of passes. The depth of each pass is calculated to remove an equal volume of material.

The spindle speed for a thread can be programmed in either RPM or CSS.

Note: The spindle speed will not increase for each pass if the thread is programmed in CSS. The initial speed calculated will be used for each pass in the thread.

When you program a thread, the system assumes a standard thread and will automatically calculate the minor diameter for you based on the pitch.

If you need to machine an acme or buttress thread, you need to select CUSTOM THREAD.

Warning: SEE Professional staff before using Custom Thread!

Select THREAD.

Prompts for the Thread event:

X BEGIN: is the X dimension or major diameter where the thread begins (diameter). Note: ID threads are also programmed using the major diameter for X BEGIN.

Z BEGIN: is the Z dimension where the thread begins.

X END: is the X dimension or major diameter where the thread will end. This should be 0, INC SET for a straight thread.

Z END: is the Z dimension where the thread ends.

PITCH: is the distance from one thread crest to the next in inches or mm. It is equal to one divided by the number of threads per inch. A 1/4-20 bolt is 1 divided by 20 = .05 inches.

# PASSES: is the number of passes (1-99) to cut the thread to its final depth (excludes spring passes).

# SPRING PASSES: is the number of passes (0-99) at the final depth.

PLUNGE ANGLE: is the angle the tool feeds into the beginning depth. The default 29.5 degrees is recommended.

SIDE: selects whether this is an I.D. (input 1, SET), or O.D. (input 2, SET) thread.

# STARTS: selects whether the thread is a single lead (input ABS SET or 1, ABS SET), double lead (input 2, ABS SET), triple lead (input 3, ABS SET), etc. (up to 10 leads). Note: Most threads will be single lead.

RPM: is the spindle speed.

TOOL#: is the tool number you assigned in the Tool Table from 1-99.

Repeat Events

The Repeat event allows you to repeat an event or group of events up to 99 times, or insert events from the Clipboard with an offset in X and/or Z.

This can be useful for a simple roughing cycle (and where a full CYCLE event is inappropriate) at increasing depths.

It is also very useful in programming rough and finish events without having to worry about adjusting the dimensions for the finish cut.

Prompts for the Repeat event:

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 (diameter).

Z OFFSET: is the incremental Z offset from event to be repeated.

# REPEATS: is the number of times events are to be repeated up to 99 times.

TOOL#: is the tool number you assign in the Tool Table for this tool, from 1-99.

CLIPBOARD: Note: See staff for instructions on how to use this feature.

Pastes 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 programs absolute zero.

Drill Events

Do not use this option. If you need to drill a hole in the center of your stock, use the Tailstock.

Bore Events

This cuts the bore to size in 1 cut! If you have a lot of material to remove use CYCLE Event.

This event allows you to bore a part using a standard boring bar. Make sure the length of the boring bar will accommodate the length of the bore.

The event tool motion will be too rapid in a straight line to the programmed X dimension, the programmed Z RAPID position, then feed to Z FINAL, then feed .01 inch towards the centerline in X to clear the tool from the part, then rapid out to Z RAPID.

Prompts for the Bore event:

X: is the diameter of the bore. Need to touch tool off inside bore to set the known value in the X axis.

Z RAPID: is the Z dimension to transition from rapid to feed.

Z FINAL: is the Z depth of the bore.

RPM/SURFACE SPEED: is the spindle speed. Enter the data and press (INC SET for RPM) or (ABS SET for SFM or SMM.)

FEED PER MIN/FEED PER REV: is the Z boring feedrate. Enter data (0.1 - 99.9 ipm/2.5 - 2500 mmpm) and press INC SET for inch per minute feed or enter data (0.001 - 0.099 ipr/0.025 - 2.5 mmpr) and press ABS SET for inch per revolution feed.

TOOL#: is the tool number you assign in the Tool Table for that tool from 1-99.

Tap Events

DO NOT USE!

Loading Programs

Note: You will need your CAD/CAM program checked by Professional Staff for verification. You can send a file via email or load it to a thumb drive. Once professional staff has approved the program, they will post it and load it to a floppy disk. Now you are ready to load program to the lathe controller.

Place your Floppy Disk into the port on the side of the control panel.

Floppy

Press MODE, and select PROG IN/OUT.

Make sure “List Supported Programs Only?” says YES. If not, press YES.

Press OPEN.

Open

If you cannot see the A: drive, use TAB to find the A: drive and use DATA FWD or DATA BACK to highlight the folder your program is in. Once the folder is highlighted, press OPEN FOLDER.

If you can see your program in the window, you can use DATA FWD or DATA BACK to highlight your program, and press OPEN FILE.

Data fwd/back

If you can’t see your program, see shop staff.

Your file will now be loaded into the memory of the controller. Press PROG and GO TO BEGIN, GO TO END, or GO TO # and select an event number, to see your program.

LOOK

At this time you can also press LOOK to see the graphical representation of your cutter paths. It gives you the ability to see your cutter paths in the X and Z planes.

Look

Look

Tool Change Reference Position

The Tool Change Reference Position is a safe position set for the cross slide and carriage to go for a tool change.

It will also go to that position at the beginning and end of a program.

These numbers are positive from absolute zero. For example: X 6.000, Z 10.000.

Tool change reference

Note: When using a live center, make sure carriage will not hit tailstock when setting the reference position.

Press MODE, SETUP, then REF POS.

Use DATA FWD or DATA BACK to highlight the X HOME STATUS.

Type in a positive number from the end of the part, for example: X 6.000.

Press ABS SET. Repeat this process for the Z, for example: Z 10.000.

Make sure this location will not collide with the tailstock, or any other part of the machine!

Do not turn on the X and Z LIMIT.

Press RETURN.

The Tool Change Reference Position must be set before you run any program, including DO ONE, conversational programs, and CAD/CAM programs.

Running Programs

Check Your Set Up

Before running your program, you need to verify that the tools are set correctly.

Press MODE, DRO, TOOL #, enter 1, ABS SET.

Now move tool #1 to Z zero on the DRO. The tip of the tool should be in the same plane as the face/end of the part in the Z axis (This position is Z 0.000).

Bring tip of the tool close to stock OD, touch tip of tool lightly on OD.

Make sure the # in the X axis on the DRO is the same number you entered for the diameter in in the X axis in the tool setup page.

Make sure you type in correct tool # when verify tools.

Repeat this for every tool to be sure each tool is set to the end of the stock, and the correct diameter.

Note: If tools are not set correctly, revert to the Setting tools page and reset tools.

Check Your Program

Check the program by pressing MODE, SET UP, and TOOL PATH.

This will process the program and display all the moves in the program, including the rapid moves.

Colors provide information about the tool path:

Position events are drawn in yellow

Rapid moves are in red

Programmed geometry is in blue.

Tool path

NOTE: If you see a line move through your part profile, something is wrong. See Professional Staff before going any further!

Running the Program

Press MODE, then RUN. If you are starting your program at the beginning, press START.  

In the event that you need to start the program somewhere besides the beginning, press START EVENT #.

Type the number of the event, then ABS. (SEE NOTE below)

NOTE: If you're not sure the event #, press MODE, PROG, GO TO BEGIN.

This will bring you to the 1st event.

Press Page FWD until you find the event you want start at and write it down. This number is what you will enter when you press START EVENT #.

The screen will prompt you Ready to begin. Press GO when ready.

WARNING: DO NOT PRESS GO! Press the TRAK-ing button. You must use the TRAK-ing feature at the start of each tool change. This will also aid in making sure the tools are set correctly.

TRAKing

Press the TRAK-ing button. Make sure it says TRAK-ing in the upper left corner of the screen. 

Traking

Turn the Z hand wheel (the one on left side of the carriage) to move the carriage and cross slide back to the Tool Reference Position.

The carriage will stop moving once it arrives at the Tool Reference position.

Now it will prompt you to Load Tool #1, Start Spindle, Press Go to Continue or TRAK-ing.

Press FWD to start the spindle, and TRAK-ing. Make sure it says TRAK-ing on the upper left corner of the screen. (Place Photo)

TRAK-ing allows you to run the program using the X and Z handles to run the program.

The Z axis handle moves through the program rapidly. The X axis handle moves through the program more slowly.

You can control the feed rate by how fast you turn the handles.

You will be able to run the whole program in TRAK-ing if desired.

If you stop turning the hand wheel, the carriage will stop. If you reverse the hand wheel, you will move backwards through the program.

Note: Make sure you run at least the first pass of each operation in TRAK-ing. This will allow you to monitor the Z depth relevant to the chuck for each tool. If you have a number of roughing passes in your program, this will allow you to monitor how deep the first roughing pass is also.

When TRAK-ing a 1 pass finishing operation, use the fine feed hand wheel (right side or X axis). This will run at slower feed rate and give you better finish.

CNC Mode

Please see Professional Staff before running in CNC mode!

If the program looks good after the first pass in TRAK-ing, you may run the program in CNC mode, if approved by professional staff.

The doors must be shut to run in CNC mode. Note: If the doors are open the machine will not run in CNC mode.

If the doors open during a CNC run machine will stop at that point and spindle will shut off.

You will be able to resume where you left of by shutting doors, pressing Spindle FWD and pressing GO on the controller or pressing the button on the pendant.

Note: Keep pendant in hand while program is running. At any time you need to stop the machine during the program, press the pendant button. Press again to restart.

Note: At any time you feel you need to stop the machine immediately, press the red emergency stop button, located on the right side door.

When operation or the program is complete, carriage and cross slide will move back to the TOOL Reference Position.

Troubleshooting

Message - Brushless Motors are not aligned.

Press MODE, SET UP, select SERV CODES, press CODE #, and enter 203. This allows the servo motors to align themselves.

Message - Could not turn hand wheels on after 100 attempts

Press MODE, SET UP, select SERV CODES, press CODE #, and enter 203. This allows the servo motors to align themselves.

Message - Tool type not set or is wrong type for that event. Edit event or change tool type in tool setup.?

Double check your program to make sure the proper Tool type has been selected.

Verify the Tool type in the program matches what has been set in the Tool library.

Also check to see if the tool numbers in the program match the tool library.

Message - Max RPM not set or machine RPM exceeded programmed RPM. Correct the fault condition and continue.?

First, verify that the MAX RPM is set for no higher than 2200 rpms, 1000 rpms if the jaws are reversed. If it has been set, look at the rpms in the program loaded in the machine and make sure you have not exceeded this set limit.

Message - Warning 5654: Data Error around event #. Cannot tool apply tool compensation on event data Check and edit event data.

You may have mistakenly entered a chamfer instead of a conrad when boring an internal profile.

Machine Shut Down

Before you shut down the machine, move the carriage to the middle of the bed, away from the tailstock, chuck, and all obstacles.

The computer on the Trak TRL 1540V is Windows based and therefore must be shut down properly in order to protect it!

Press the Windows logo.

Windows logo

Press SHUT DOWN.

Shut down

Press YES and wait for a message to appear on the screen. It will say “It is now safe to turn off your computer”.

Remove the floppy disk, and flip the toggle switch located on the right side of the pendant to the “DOWN” position. Return floppy to professional staff.

Toggle off

Rotate the ON/OFF switch located at the back of the machine to the OFF position.

Make sure the lathe is clean and checked by shop staff before you leave the shop.




Keywords:trak, lathe, tutorial instruction, cnc, 1, 2   Doc ID:83423
Owner:Jay B.Group:TEAM Lab Documentation
Created:2018-07-06 11:06 CDTUpdated:2018-10-19 10:54 CDT
Sites:TEAM Lab Documentation
Feedback:  0   1