TRAK 2op Machine Guide

Standard start up procedures for the Southwestern Trak 2nd operation machining center.

 

 

Overview

  • The Trak 2op machine is intended for light to medium size work.
  • The table size is 18”(457 mm) x 15”(381 mm) with machine travel limits as follows: X axis is 14” (355 mm), Y axis is 12”(304 mm), and the Z axis is 17”(431 mm).
  • It has a maximum spindle speed of 6000 rpm and a maximum rapid feed rate of 600 ipm.
  • If you need a machine that is capable of doing larger work, consider using the TMC 7. 

overview

 

 

TMX controller

The TMX controller has some of the same capabilities as the EMX controller (Eisen mills) and the SMX controller (Trak DPM's).

 

It's capable of programming conversational programs (PT4) along with running GCD files generated from a CAD program and loaded to the machine from a thumb drive.

control

Machine Start up

1. Turn the Main Power Switch in the back of the machine from the "OFF" position to the "ON" position as shown in the pictures below.

off     on

2. Be sure the red E-Stop button, located at the top left corner on control panel, is pulled out.

3. When the orange ProtoTRAK TMX screen prompts up, you'll notice the top of the screen displays "servo off."

4. Press the green button at the top right hand corner of the control panel to turn servos on.

5. You will hear the lube pump start up and the prompt will change at the top screen to "servo on".

 servo off   servo on
 
 
Homing the machine
Homing the 2op sets the machine home reference positions in the X,Y and Z axis's and will have to be done at each machine start up.
 
The head will move all the way to the right during the homing process, so you want to make sure the coolant lines are clear between the right side of the machine and the spindle as shown in the pics below.
 
wrongcorrect
Just like the X axis, the Y axis will move all the way back toward the operator with the door closed, so the vise and vise handle can not stick out past the table or it could cause damage to the door.
If the vise handle is still attached, remove it completely to avoid any damage to equipment during the homing process and/or running the program.
Normally, you should not have to remove the vise since it is centered on the fixture plate, but if something doesn't look right or you are not sure, see staff!
 
                                      vise handle                                      
Press the SET Home soft key. The next screen will show green message box with the message "Ready to begin. Close door and press go when ready", as shown in the center picture below. 
 
A green box will appear with the message "Please wait" during the homing process as shown in the pic below on the right.
       
set home                
 
  
When the homing process is finished, the modes will appear on the control screen as shown below.
 
mode screen
 
 
 
 
Navigating the control panel
 
control panel
 
 
 
EHW, Resolution and Axis buttons                     
  • These buttons allow you to move the axis selected in DRO or SETUP modes.
  • To do so:
    1. Select a resolution (speed) button
    2. Select the axis you want to move.
  • This will allow you to move the axis selected with the Electric Hand Wheel (EHW).
                                                                                                                                                                                                                                                                                                                                         
ehw   resolution  axis 
 
 
EHW tag 
The resolution and the axis buttons selected will light up and a red EHW tag will display on the screen, next to the selected axis as shown in the picture below. 
 ehw tag                      
 
Zeroing each Axis
To zero an axis or to set an axis to a number, you must be in the DRO mode. Next, select the axis you want set by pressing the axis button.
 
The axis should be highlighted in yellow as shown in the picture below. Now, type the number you wish to enter and press ABS set. 
 
If you press the wrong number or the wrong axis button, press the Restore (RSTR) below the mode button and it will bring you back to where you were before you started.
zero axis
 
 
 
 
 
ProtoTRAK TMX Screen in DRO Mode
DRO Functions
Soft Keys in DRO Mode:
    • Return ABS 0: initiates rapid move to machine X,Y absolute 0 and Z to the tool change height position.
    • REF: allows you to choose ABS, INC, BALL LOCK or machine HOME reference locations.
    • OVERRIDES: allows you to adjust spindle speed and feed rate, using the electronic hand wheel (EHW)
    • SPIN SPEED: allows you to set rpm manually by pressing the spindle speed soft key, typing the desired RPM and the pressing ABS set.  
Programming
 
Press the MODE button on the right side of the control panel. 
 
Press PROG EDIT.
prog edit
 
The screen will go to the program screen (see lower left pic). You will notice PROG in the upper left hand corner (see below pics).
 
Type in Program Name (if needed) and press ABS SET to save.
 program name                      prog number
 
 
  • Ball lock locations are used to save part zero to allow a quicker set up next time you run the same part, mainly used for production runs.
  • If you don't use the ball lock location, press ABS SET to curser down. You can also move the curser up or down using the Electronic Hand Wheel.
  • Indexer prompt is only used when using an indexer. You will not be using an Indexer so press the NO soft key or turn EHW to go to Event 1.
  • A green box will appear with the message "Select an event". The events are listed at the bottom of the screen. To select an event, press the soft key below each event. As shown in the pic below.
ready to prog
 
 
Events  
  • POSN DRILL

Will move the table to a location you define at a rapid feed rate. Used for location only!

position 
 
  • DRILL  
A green box will prompt you to select 1 for drill, 2 for bore or 3 for tap, then press ABS SET. (Note: You will not use the tap prompt.)
Event selected will show up right of the "DRILL,BORE,TAP" parameter. An example is shown below in the pic on the right.
drill             drill event
    • Drill - X and Y location of the drilled hole.
      • Z rapid - is location where rapid feed will stop and where the Z feed rate starts (usually set at .100 above the part). 
      • Z end - is the depth of the hole.
      • # Pecks - is the number of pecks the Z axis will do when drilling the hole.
      • RPM - is spindle speed during drilling.
      • Z feed rate - is the feed rate during drilling.
      • TOOL # - designated for the drill.
      • TOOL DIA -  is diameter of designated tool.
    • Bore - X and Y location of bored hole.
      • Z rapid - is where rapid feed stops and Z feed rate starts(usually set at .100 above the part).
      • Z end - is the bottom of the bored hole.
      • RPM - is spindle speed.
      • Z feed rate - is the  Z axis feed rate during boring cycle.
      • TOOL # - is number of the designated tool for boring.
      • TOOL DIA - is the diameter of the boring tool. 
    • Tap  - X and Y locations for hole to be tapped. (Warning: Do not use!)
      • Z rapid - is where rapid feed stops and Z feed rate starts(usually set at .100 above the part).
      • Z begin - is where you want the tap to start.
      • Z end - is the bottom of the tapped hole.
      • Pitch - is the pitch of the thread to be tapped. 
      • RPM - is spindle speed. 
      • TOOL # - is given for that tool.
      • Tool DIA - is the diameter of the tap.
 
                
BOLT HOLE 
This event allows you to program a bolt hole pattern without needing to compute and program the position of each hole.
 
bolt hole

 

Prompts for the Bolt Hole event are as follows:

  • Drill=1, Bore=2: selects whether the hole is to be drilled or bored.

(You will also have the choice: Tap = 3. Warning: do not use this option.)

  • # Holes: is the number of holes in the bolt hole pattern.
  • X Center: is the X dimension to the center of the bolt hole pattern.
  • Y Center: is the Y dimension to the center of the bolt hole pattern.
  • Z Rapid: is the location where rapid feed will stop and where the Z feed rate starts (usually set at .100 above the part).
  • 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 axis (that is, 3 o'clock) to any hole; positive angle is measured counterclockwise from 0.000 to 359.999 degrees, negative angles measured clockwise.
  • # PECKS: Is how many times the Z will move up and down during the drilling cycle. Note: You can change the peck setting by pressing the ? soft key.
  • VARIABLE is where the drill goes to successfully smaller depths and comes out of the hole between each peck. (This is the default setting.)
  • FIXED is where the drill goes to the same incremental depth and comes out of the hole between each peck.
  • CHIP BREAK is where the drill goes to the same incremental depth but pauses briefly at each depth, instead of coming out of the hole.
  • RPM: is the spindle RPM for the event. INC SET will use the RPM of the previous event.
  • Z Feed rate: is the drilling feed rate.
  • Tool #: is the tool number you assign.
  • Tool Dia: Diameter of the cutting tool.
 
MILL EVENTS
 
This event allows you to mill in a straight line from any one X,Y,Z 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 are as follows on the screen below.
 
mill 1
  • 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 location where rapid feed will stop and where the Z feed rate starts (usually set at .100 above the part).
  • Z Depth: Is the depth of cut.
  • 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 (that must lie in the same plane for part geometry programming).
  • Tool Offset: is the selection of the tool offset to right(1), offset to left (2), or tool center--no offset (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.
  • Z Feed rate: is the Z feed rate from Z Rapid to Z begin.

Use the EHW to scroll down and enter the rest of the information listed below.

  • XYZ Feed rate: is the milling feed rate 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.
  • Tool Dia: Diameter of the cutting tool. 
  • Continue: Tells the controller if this event is continuous to the next event. For example: if you press1 for yes, you will not have to enter data in the next event for X and Y begin, Tool Offset, Feed rate and tool #.
 
  
ARC event
This could be any part of a circle.
Like the mill event, the data you provide on the screen will allow the TMX controller to calculate the tool path.
 
arc 1
 

Prompts for the Arc event are as follows from the screen above:

  • 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 location where rapid feed will stop and where the Z feed rate starts (usually set at .100 above the part).
  • Z Depth: is the depth of cut.
  • 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 (which must 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, looking from the front for a vertical plane, or looking from the right for a vertical YZ plane.

Use the EHW to scroll down and enter the rest of the information listed below.

  • 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.
  • Z Feed rate: is the Z feed rate from Z Rapid to Z Begin.
  • XYZ Feed rate: is the milling feed rate 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. 
  • Tool Dia: Diameter of the cutting tool
  • Continue: Tells the controller if this event is continuous to the next event. For example: if you press1 for yes, you will not have to enter data in the next event for X and Y begin, Tool Offset, Feed rate and tool #.
 
POCKET PROFILE
 
This event selection gives you a choice between:
CIRCLE POCKET, RECTANGLE POCKET, CIRCLE PROFILE, RECTANGLE PROFILE and FACE MILL.
 
pockprof
 
  • 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 will begin away from the wall to be finished, arc into the finish cut, 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.
The following are all options within POCKET PROFILE: 
  • CIRCLE POCKET
Press the CIRCLE PCKT soft key if you wish to mill a circular pocket.
Prompts for the CIRCLE POCKET as shown below.
 
circle pocket 1

 

  • 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 location where rapid feed will stop and where the Z feed rate starts (usually set at .100 above the part).
  • 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 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 plunge will machine straight down Z to the appropriate Z depth. The zigzag ramp will move in a zigzag pattern to depth.
  • 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.

Use the EHW to scroll down and enter the rest of the information listed below.

  • FIN RPM: is the spindle RPM for the finish cut.
  • Z Feed rate: is the Z feed rate from Z rapid to Z end.
  • XYZ Feed rate: is the milling feed rate in in/min from .1 to 150, or mm/min from 5 to 3810.
  • Fin Feed rate: is the milling feed rate for the finish cut.
  • Tool #: is the tool number you assign.
  • Tool Dia: Diameter of the cutting tool.
 
 
RECTANGULAR POCKET
Press RECTANGLE POCKET soft key if you wish to mill a rectangular pocket (all corners are 90 degree right angles and the sides are parallel to the X and Y axes).
 
The prompts for the rectangular pocket as follows below.
rect pocket 1
  • 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 diagonal to X1; incremental is from X1.
  • Y3: is the Y dimension to the same corner as X3; incremental is from Y1.
  • Z Rapid: is the location where rapid feed will stop and where the Z feed rate starts (usually set at .100 above the part).
  • 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.
  • # 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 zigzag 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.

Use the EHW to scroll down and enter the rest of the information listed below.

  • 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.
  • FIN RPM: is the spindle RPM for the finish cut.
  • Z Feed rate: is the Z feed rate from Z rapid to Z end.
  • XYZ Feed rate: is the milling feed rate in in/min from .1 to 150, or mm/min from 5 to 3810.
  • Fin Feed rate: is the milling feed rate for the finish cut.
  • Tool #: is the tool number you assign.
  • Tool Dia: Diameter of the cutting tool.
 
 
 
CIRCLE PROFILE
Press the CIRCLE PROFILE soft key if you wish to mill a circular frame.
 
Prompts in the Circle Profile event as listed below.
 
circle pocket 1
 
  • 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 location where rapid feed will stop and where the Z feed rate starts (usually set at .100 above the part).
  • Z End: is the Z dimension to the bottom of the frame; incremental is from the previous event.
  • Radius: is the finish radius 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:(NOTE: keep Z Rapid small, but higher than your clamps).
  • 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.

Use the EHW to scroll down and enter the rest of the information listed below.

  • FIN RPM: is the spindle RPM for the finish cut.
  • Z Feed rate: is the Z feed rate from Z rapid to Z end.
  • XYZ Feed rate: is the milling feed rate in in/min from .1 to 150, or mm/min from 5 to 3810.
  • Finish Feed rate: is the milling feed rate for the finish cut.
  • Tool #: is the tool number you assign.
  • Tool Dia: Diameter of the cutting tool.
 
 
RECTANGLE PROFILE
Press the RECTANGLE PROFILE soft key if you wish to mill a rectangular frame (all corners are 90 degree right angles).
 
Prompts for the RECTANGLE PROFILE as follows below.
 
rect prof1
 
  • 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 diagonal to X1; incremental is from X1.
  • Y3: is the Y dimension to the same corner as X3; incremental is from Y1.
  • Z Rapid: is the location where rapid feed will stop and where the Z feed rate starts (usually set at .100 above the part).
  • 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).

Use the EHW to scroll down and enter the rest of the information listed below.

  • 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.
  • FIN RPM: is the spindle RPM for the finish cut.
  • Z Feed rate: is the Z feed rate from Z rapid to Z end.
  • XYZ Feed rate: is the milling feed rate in in/min from .1 to 150, or mm/min from 5 to 3810.
  • Fin Feed rate: is the milling feed rate for the finish cut (if programmed).
  • Tool #: is the tool number you assign.
  • Tool Dia : Is the diameter of the cutting tool.
 
 
 
FACE MILL
Press FACE MILL soft key if you wish to face or clean up the top of a work piece.
    • 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  as follows below.
 
face mill 1
 
  • 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 diagonal to X1; incremental is from X1.
  • Y3: is the Y dimension to the same corner as X3; incremental is from Y1.
  • Z Rapid: is the location where rapid feed will stop and where the Z feed rate starts (usually set at .100 above the part).
  • 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 there 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 spindle RPM for the finish cut.

Use the EHW to scroll down and enter the rest of the information listed below.

  • Z Feed rate: is the Z feed rate from Z rapid to Z end in in/min from .1 to 700, or mm/min from 5 to 17780.
  • XYZ Feed rate: is the milling feed rate in in/min from .1 to 800, or mm/min from 5 to 20320.
  • Fin Feed rate: is the milling feed rate for the finish cut.
  • Tool #: is the tool number you assign.
  • Tool Dia: Diameter of the cutting tool.

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%.

 
Loading Files from a Thumb Drive
 
Place your thumb drive into the USB ports located on the right side of the machine.
 
thumb drive
 
 

1.  Press Prog in/out soft key. 

You should see the list of programs store on the memory device. 
prog button 
 
2.  Type in the program number and press the open soft key. 
progtype  
 
3.  It will ask you if it is a .PT4 or .GCD, press what ever the program is listed on the display screen.
PT4GCD
  
4. Press YES to overwrite the current program.
Pressing NO takes you back to the GCD/PT4 screen.
overwrite message
 
5.  Press NO to use existing offsets
keep exsisting offstes
 
 

Tool Setup and Tool Holders

The 2op requires the use of BT30 tool holders with retention knobs which are found in the green tool boxes provided for each of the 2op machines.

  • Keyless and Key chucks - drills, spot drills, edge finders, no endmills

chucks

  • Collet Chucks - drills, endmills, ground shank tooling.

collet holders

  • Endmill holders - ground shank tooling with flats

endmill holders

  • Tool mounting fixture - Used to tighten tool holders

mounting fixture

  • Tool setter - used to set Z offsets in the tool table

toolsetter

Endmills with flats

The first tool holder of choice for an endmill with a flat can be seen below. This tool holder has a setscrew intended to clamp onto the flat of the endmill shank. NEVER USE A KEYLESS CHUCK WITH AN ENDMILL!

 
Begin by removing the setscrew to align the flat on the shank with the hole.

Finally, use the tool holding fixture in the vise to tighten the setscrew.

Tools with a round shanks

For an endmill with a round shank, use a collet holder seen below. You may also use the collet holders for drills, spot drills, and any other tooling with a round shank. AGAIN, NEVER USE A KEYLESS CHUCK WITH AN ENDMILL!

Begin by finding a collet that properly fits your tool. 

If needed, place the selected collet into the holder. To remove a collet from the holder, push the bottom of the collet to the side until it pops out. While placing a collet into the holder, repeat the same process in reverse.

The face of the collet should be in line with the face of the holder as seen below.

Finally, place the tool into the collet and tighten it down. Use the tool holding fixture and wrench found in the green toolbox to tighten the collet, as seen below.

Drills, Spot Drills, and Edge Finders

For all drills and edge finders use either a keyed or keyless chuck. NEVER PLACE AN ENDMILL INTO A CHUCK!

While placing a tool into a chuck ensure the tool is placed as far down as it can go. The first image (left) is incorrect and the second image (right) is correct. Failure to do so can cause incorrect tool offsets.

Tighten a keyless chuck by placing it into the tool holding fixture and using the wrench found in the green toolbox. Note: Not all keyless chucks have the ability to be tightened by a wrench.

Setting tools

Manually load tool into the spindle by pressing and holding the white button while lining up the drive dogs on the spindle with the notches in the tool holder. 

Hold the tool holder until it is seated then you can release the white button.

loading tool         

Press SET-UP mode soft key 

Next press the tool table soft key and that will bring you to the tool table screen shown in the pic below at the far right.

set up modetool tabletool table tool #

Notice the tool numbers from the program are already highlighted in red. 

NOTE:

    • When you upload a GCD file from a CAD file, you will not need to type in the tool diameters in the tool table. The tool diameters are already in the program. (GCD Example below on the left).
    • When programming at the machine (PT4 file), the tool diameters will transpose from your program to the tool table as long as you as create the program first. (PT4 example below on the right).

tool table tool #Tool dia transposed

  •  Grab the tool setter out of the wooden case in the green tool box and place it on the solid jaw of the vise with the indicator facing you as shown in the pic below to the far left.
  •  Position the tool approximately ¼” above the tool setter using the EHW. Press the .0002 resolution key and then the Z axis button if you haven’t already, shown in the center pic below.
  •  Slowly bring the tool down onto the tool setter (using the EHW) until the small dial and the big dial are at 0 as shown in the picture at the far right below.

tool settertool positiontool setter references

  • If the cursor is still on the tool diameter, use the right arrow soft key to move the cursor to the Z offset column or just press ABS set (shown below in the pic on the left). 
  • Now press ABS SET. This will put the value into the Z offset for that Tool #. The cursor will now move to the Z modifier column (shown below in the pic on the right).

cursor                 move cursor

  • Z MODIFIER is used to fine tune your Z depths. Positive values will cut shallower and negative numbers will cut deeper. You will rarely use this function so press ABS set or arrow over to tool type.
  • TOOL TYPE adds a description of the tool along with the tool number. It's not necessary to use, but it is helpful.
    • Follow the prompts in the green box as shown In the pic below in the center. The pic on the right shows an example of the tool type after following the prompts.

    setting z offset     z modifier     tool type

    • Use the EHW to raise the tool away from the tool setter in a comfortable position to remove the tool from the spindle.
    • Firmly hold the tool holder with your right hand while pressing the white button with your left-hand to manually remove the tool. 
    • Place the next tool into the spindle and repeat the process to set the Z offsets for all the tools in your program using the steps noted prior.
    • After all the tools are set, press the return button to get back to the set up page.

 

 

 

Loading tools into the ATC

  1. Organize your tools in the order they appear in the program.
  2. Manually place tool 1 into the spindle.
  3. Now press Load Tools soft key as shown below in the pic on the far left.
  4. A green box will appear on the screen, prompting you to "Press go to move ATC to front" as shown in the pic on the right.The ATC will move forward from the back of the machine.

  load tools soft key     atc front    

   Read prompts carefully! Failure to do so could cause damage to tools and the machine.

ATC messages

  • Tool in ATC - Moves tool from the spindle into the ATC.
  • Tool out ATC - Moves desired tool from ATC to the spindle. NOTE: spindle must be empty prior.
  • Load Man Tool - Allows user to add tool manually to the spindle and updates tool status to that tool number. Primarily used for tools numbered 9 and above.
  • Unload Man tools - Allows user to remove the manual tool added and update the tool status line.

Read the prompts carefully in the green box. 

In the example pic below, you would press Tool in ATC and enter the ATC location you want the tool to be placed (if it’s tool 1, press 1) and press go. The spindle will lower to the tool change position.

ATC message page

A green box will appear asking you, are you sure the tool change spot is empty?

    • If it is, press the yes soft key. A green box will appear prompting you to press the "GO" button to complete the tool change as shown below in the pic in the middle.
    • Once that tool is placed into the ATC, a blue dot will occupy the spot in the ATC you just placed the tool into as shown in the pic on the right.
    • Continue with this process to place all tools used in your program into the ATC.

   Empty spot   tool go   blue dot

Note: You must have tool 1 loaded into the spindle before you start the program!

 

 

 

Setting Z

1.  Place tool into the spindle from the ATC (usually tool #1 because it's the 1st tool in the program). 

2.  Now go to the DRO mode and make sure it says tool 1 in the tool # box at the top of the screen as shown in the pic below.

tool 1 

3.  Using the EHW, bring the tool down within a 1/2" from the top of your stock. 

tool position 

4.  Place a piece of paper on top of the stock.

5.  Press the .0002 resolution and slowly bring the tool down using the EHW in the Z axis. 

6.  Lower the tool until you can't wiggle the paper between the tool and the part.

tool touch off

7.  Press the resolution button that is lit up, first. This will cancel out the feed and you will notice that the lights on both buttons used, will turn off as shown in the pics below.  

0030         axis lights

8.  At this point, press the Z axis button.(the Z axis should be highlighted in yellow, as shown in the pic below). 

Now press ABS set. This will set the Z zero at the top of your stock.

set z zero

Running the program

1. Load the program 
2. Set the Z offset for each tool into the tool table
3. Place the tools into the ATC
4. Secure the stock into the vise and find the origin of your part 
5. Set the Z zero with tool #1
NOTE: If the steps have not been completed as stated above, the RUN button on the mode screen will be shadowed out as shown in the picture below on the left.
Once these steps above are completed in the order listed above, you can now run the program.
Make sure the door is closed(it will prompt you to close the door on the screen if open).

run shadowed     run ready

  • Press the RUN button. You will see Start and Start Event # buttons as shown in the pic below.
    • Start will start you at the beginning of the program. 
    • Start Event # allows you to start at a selected event # in your program as long as you know the event #.
  • You will select the START button. The next screen you will see is the pic below at the right.

start      traking

 

 

 

TRAKing

You will use TRAKing at the start of every program and every tool change.

TRAKing is a safety mechanism that to make sure that you have the Z zero set correctly at the start of the program and at each tool change.

  • The user will slowly bring the tool down until it makes a small chip at the top of the stock.
  • Now check the Z axis to make sure the it is reading 0. If that number is significantly off, stop the program and reset the Z zero in the DRO mode for that tool #.

 NOTE: If it continues to be off, the user may have to reset the Z offsets in the tool table for each tool again. 

Press the TRAKing soft key. On the next screen you will see in the upper left hand corner of the screen that you are in the TRAKing mode as shown in the pic to the right below.

traking highlighted    traking screen hilighted

TRAKing allows you to control the feed rate by turning the EHW.

You can also change the speed that you TRAK by pressing any one of the feed resolution buttons just to the right of the EHW.

It is suggested to use the .002 inch resolution to have more control as shown in the pic below.

traking res

After confirming that the Z axis is set correctly, the user can now run in CNC mode.

  • Press the Cycle stop button as shown in the pic in the lower left. Now you should see CNC run next to TRAKing as shown in the pic in the lower middle pic.
  • Press the CNC run soft key and press Cycle GO.
  • The program will start running in full CNC mode.

NOTE: Please be be aware where the Cycle stop button is in case something should go wrong. This will stop the program immediately.

You can go back to TRAKing at anytime by pressing Cycle stop and TRAKing.

traking to cnc   traking message   go cnc

The user has the ability to run the whole program in TRAKing if they chose to do so. 

  • Once the program gets to a tool change in the program while TRAKing, the machine will take over automatically and perform the tool change. 
  • Once the tool change is complete, the user can resume TRAKing using the EHW.

If the user is in CNC run mode at a tool change, press Cycle stop. 

  • Once the tool change is complete, the user can now press the TRAKing button and TRAK the tool to the top of the stock and check the Z 0 as stated earlier. 
  • Once the user is satisfied with the Z setting, they can continue running in TRAKing or go to CNC run mode.

 

 

Saving a file to a thumb drive

  • Place a thumb drive into one of the USB ports on the right side of the machine.
    • Press the MODE button if you are not already in the mode screen.
    • Press Prog IN/OUT soft key as shown in the pic below on the left.
    • You will see that your program number will transpose in the program name box as shown by an arrow in the pic below on the right.
    • Now press the SAVE soft key highlighted in the pic on the right below.

prog soft key     press save

Press the SAVE soft key as highlighted below in the pic on the left.    

Now you will see the program number added to the thumb drive as shown by the arrow in the pic below on the right.

save button    program listed

 

 

Removing tools from the ATC

Manually remove the tool currently in the spindle by firmly holding onto the tool and then pressing the white button located on the spindle head as shown in the pic below.

spindle tool

Press SET-UP soft key. Press LOAD TOOLS soft key. Press GO to get the ATC out toward the front.

set up button unloading tools   atc forward           

  • Read the prompts carefully and follow those prompts to remove the tools out of the ATC and into the spindle.
  • In this case, press tool out ATC, now type 2 to remove tool 2 and if the spindle is physically clear press yes as shown in the pics below from left to right.
  • Once they are loaded into the spindle, manually remove them as stated above.
  • Repeat the process until all the tools are removed from the ATC.

tool removal wm rtm

 

Place the tool holding fixture in the vise and remove the tooling from the holder as shown in the pic below and place the tools and holders back into the green tool box.

holder

 

 

 

Cleaning the machine

Use the blue brush, located in the green tool box, to brush any chips from the vise and table down into the chip pan as shown in the pic below.

chip pan

 

  • Use a rag to wipe down the inside of the machine free of smaller chips and coolant.
  • Coolant is a water based solution, so it's very important to make sure all the coolant is wiped off of machined surfaces to prevent any rust happening.
  • Now spray the surfaces with WD-40 as another level of protection against rust.
  • Lightly lift and pull on the handle of the chip pan drawer to access the inside to remove the chips.

 

chip pan access

Use a brush and a dust pan to remove the chips from the chip pan and place the into a metal chip bin(s) located in the lab as shown in the pics below.

sweeping chips dumpster

 

 

 

Shutting down the machine

Press the MODE button if not already in the MODE screen.

Press RSTR button as shown in the pic below.

rstr11

 

  • Press SHUT DOWN button.
  • Read the message on the screen and press YES.
  • Go to the back of the machine and flip the main power switch from ON to OFF.

shut down sd message turn off

 

Have staff check your machine, tool box and work area to make sure it is clean and tools are in good working order.


Keywords:
cnc, 2 op, trak, machining center, mill, 3 axis 
Doc ID:
96793
Owned by:
Jay B. in ECB Shops Documentation
Created:
2019-12-26
Updated:
2024-12-17
Sites:
ECB Shops Documentation
Clean URL:
https://kb.wisc.edu/trak-2op