Import a DXF file And Machine The Part Geometry

  1. Get 2 approximately 3”x 3” x.5” pieces of stock. Mount one of them in the vice, and then clamp the second firmly on top of it, approximately lining up the edges.
  2. Erase old program in memory (if one exists):
  • Hit MODE to get to main menu - EDITERASE PROG - YES

     3. Make sure the mouse is plugged in and functioning. Plug flash drive containing DXF file into ProtoTRAK machine. Alternatively, you can use a computer to drag and drop the DXF File into the appropriate mill folder in the “mshop_files” folder on the Thayer FS “Common” drive. The file name for this tutorial is “dxf example part”

     4. Open the DXF file 

  • Hit PROG IN/OUT- OPEN
  • Select the appropriate file[1] using the mouse or touch keys, and then hit OPEN FILE.
  • Your DXF should appear on the screen with a list of options at the bottom. Select the file and press OPEN FILE. Press CONTINUE and then YES when asked if you want to close gaps[2].

     5. Set program absolute zero

  • Select A to define the zero by an “Intersection of Two Lines and/or Arcs.”
  • For this example, set the zero to be the top left corner of the part. With the mouse, select the left vertical line and the top horizontal line. A boxed red “X” will show you where the program zero has been set.

     6. Program the two holes

  • CONTINUE- CONTINUE[3]
  • “Select Event” should appear, with a list of different operations at the bottom.
  • Click DRILL once and then left click both circles. They should turn purple.
  • Click DRILL again to finish creating drill events (the holes will both turn light blue).

     7. Program the profile cut

  • Click PROFILE and YES when it asks to chain.
  • Select the top line first and then the small arc to the right. It should automatically outline the rest of the profile for you and turn light blue, indicating that it is set.

     8. Tool setup

  • Click END DXF- YES to exit the DXF setup. The mouse is no longer needed.
  • MODE- SET-UP- TOOL TABLE to bring up the list of tools for this program[4].
  • DATA DOWN to highlight the diameter field of Tool #1
    • Enter drill diameter (0.25) - ABS SET- 1 (under tool type to select “Drill”) -ABS SET.
  • Tool #2 diameter field should now be highlighted. Enter end mill information:
    • Enter tool diameter (ex. 0.25) - ABS SET- 4 (for finish end mill) - ABS SET
    • NOTE: The tool diameter here must be entered precisely in order for the machine to offset properly. If using a 1/4” end mill, 0.2500 must be entered, etc.[5]
  • MODE to get back to main menu.

     9. Define critical parameters in events

  • The drill/profile events still have not had certain parameters set. You will now go through each event to make sure the necessary parameters are satisfied.
  • PROG- GO TO BEGIN
  • Event 1 shows up on the right, indicating that it will first perform a position drill.
    • DATA FWD past “X end” and “Y end”.
    • Enter (2500)for RPM
    • Under “Tool #”, enter 1-ABS SET. The drill has now been set.
  • Event 2 shows the second position drill. Repeat the previous step to set the drill again.
  • Event 3 shows the beginning of the profiling.
    • DATA FWD to the “Tool Offset” field.
    • Since we are profiling clockwise, we want the tool to offset to the left of the actual line. Enter 2-ABS SET
    • For the “FIN CUT” field, leave blank and ABS SET
    • Enter (3000)for RPM
    • Enter 6-ABS SET for “Feedrate”[6]
    • Under Tool #, enter 2-ABS SET to use the correct end mill you previously programmed.
  • Event 4 shows “A.G.E. Mill”. Note how “OK” is displayed at the top right. No parameters need to be changed here. PAGE FWD to go to the next event.[7]
  • Event 5 shows “A.G.E. ARC” and also has “OK” displayed. PAGE FWD until you reach Event 13.
  • If the program continues past Event 13, or if it does not display “OK” for events 4-13, talk to a TA.
  • After Event 13, the end of the program has been reached and we can now run it.

     10. Zero the machine

  • Knowing that the program zero has been set to the upper left corner of this part, set the machinezero so that you have enough room to create the part on the material.
  • MODE- DRO to enter the digital readout screen.
  • Load the SPRING-LOADED CENTER, and position the spindle about 1 inch above the workpiece. Move the spindle so that it is in the top left corner of the part, between .5 inches and 1 inch from the edges.
  • Zero the X and Y axis
    • X - type 0- ABS SET
    • Y- type 0- ABS SET
  • When we are profiling, we will need to know how deep the endmill is into the part, so we need to set a Z-zero as well.
    • Load the 1/4-inch endmill
    • Touch the tip of the endmill to the top of the workpiece
    • Z- type 0- ABS SET
  • MODE to get back to main menu

     11. Test run

  • Re-Load the spring-loaded center, and position it about 1 inch above the surface of the workpiece. This will allow you to accurately see if the machine follows the correct profile.
  • Hit RUN- TRIAL RUN[8]
  • MAKE SURE THAT THE TOOL WILL NOT CRASH INTO THE CLAMPS.Move the clamps if necessary to give the machine a clear run through the part.
  • Close the guard doors, and press GO. Ensure that the machine follows the correct path.
     

     12. Actual Run

  • RUN- START - GO
  • “Ready to begin… Press GO when ready” should appear. Press GO or hit the button on the controller.
    • It will ask you to load tool #1. Load the center drill. Make sure the tool is above the material and press GO.
    • Note: use the “STEP Z” function to adjust the height of the spindle as necessary to change tools. HOWEVER, do not STEP Z too close to the material, or you will crash the tool.
    • The tool will move to the location of the first hole. “Set Z” indicates that the hole is ready to be drilled. Drill a spot hole.
    • Press GO to move to the next hole. “Set Z” appears again. Drill another spot hole.
    • Stop the program, and press mode to exit to the home screen. Then repeat these steps once more, except drill entirely through both pieces of stock using the 1/4-20 tap drill.
    • Stop the program, and press mode to exit to the home screen. Then repeat steps 1-4 once more, with the following exceptions:
      • Use a 1/4-inch clearance drill
      • Drill ONLY through the top plate - do not drill through both plates.
    • Stop the program, and press mode to exit to the home screen.
    • Re-run the program.
    • It will ask you to load tool #1. Load the spring-loaded center. Make sure the tool is raised above the material and press GO.
    • The tool will move to the location of the first hole. “Set Z” indicates that the hole is ready to be tapped. Make sure you turn the spindle OFF.
    • Place the tap handle and a 1/4-20 tap through the clearance hole in the top plate and into the hole in the bottom plate. DO NOT remove the top plate.
    • Lower the spring-loaded center into the hole in the back of the tap handle to keep the handle straight.
    • Tap the hole all the way through.
    • Remove the tap handle, raise the spindle, and press GO to move to the next hole.
    • Repeat steps 11-13 for the second hole.
  • Remove the tap handle and raise the spindle. Press MODE - DRO to enter the digital readout screen, and move the spindle out of the way.
  • Screw the top plate onto the bottom plate
    • Acquire two 1-inch 1/4-20 machine screws from the drawers in Couch Lab
    • Use them to screw the top plate onto the bottom plate.
    • When the top plate is secure to the bottom plate, remove the clamps so you can move on to cutting the profile.
  • Cut the profile
    • Start the program from the profiling event.
  • Hit RUN - START EVENT #-type 3- ABS SET
    • Press GO. The machine will prompt you to load the end mill and start the spindle. Do so.
    • SHOW PATH to watch the next part of the run.
    • Press GO and the end mill will move to the start of the profile.
    • “Set Z” appears. Gently drill down to Z=-0.125. Lock the spindle
    • Press GO and the machine will begin outlining the part. Watch the blue outline to make sure it will cut properly.[9]
    • When “Check Z” appears, lift the tool.
    • Hit GO and the end of the run is indicated. Hit MODE.
    • Repeat the above steps, moving Z down another .125 (or less as necessary) each time, until you have cut the part out of the top piece of stock. Avoid cutting more than .1” into the bottom plate.
    • Remove the screws, and remove the newly cut part from the waste stock.
  • Your part is ready for inspection.

[1] If the flash drive does not appear, unplug it and exit to the main menu (MODE). Plug back in and wait a moment before trying to open the file again. You can also try searching for the folder at the top of the PROG IN/OUT section.

[2] If your drawing does have gaps in it, the ProtoTRAK could attempt to close them at this point. For this DXF File the gaps are invisible, but they are enough to mess with the mill’s programming capability. Any visible gaps should be fixed in your drawing software, not in the ProtoTRAK mill.

[3] Here you can add more lines or points to the drawing on the screen. However, it is easier to do this beforehand rather than on the ProtoTRAK screen.

[4] For this program, only two tools are being programmed: the drill and the end mill. Setting up drill tools will serve as good reminders when you are actually running the program.

[5] The diameter of the drill tool is not crucial, since it will center over the hole and you can use a center drill or any size bit. The diameter of the end mill is crucial, and must not be overlooked. The machine uses this information to offset the end mill the correct distance from the edge.

[6] This is how fast it will mill around the part. You can speed this up or slow this down while running the program, but 6 is a good starting point.

[7] When using the profile tool, the computer will automatically calculate the start/end points and paths of all the individual mills/arcs it has to make in order to get the profile of your part. Events 4-13 are all of the actual events needed to profile the part. The initial profile event (Event 3) is the only one that needs to be defined.

[8] Make sure you have proper clearance since the machine will run through the program extremely fast. If this is not done correctly, the machine will forcefully hit its limits.

[9] The tool will automatically offset to the left of the path of your DXF, even though it appears to be going right over it.

⬆︎