What is the proper programming format for a tapered or 4-axis profile that requires manual wire threading of an angular start hole?

by | Apr 1, 2020 | Small Hole

This is a great question since an angular start hole is a situation that commonly occurs in mold tooling lifter pocket or ejector pin details. As part of this process, a position for manual wire threading needs to be determined within the profile, and an M01 stop point should be created within the NC program at this point.  When processing with a tapered start hole, the angular start hole position needs to become part of the program so that it is included within the program cutter compensation (G41/G42) line.

If the angular start hole location is not part of the utter comp (G41/G42) movement, a machine alarm can occur. In the case of 4-Axis programs, cutter comp may not be activated properly if the U/V axes are not vertical, leading to improper size and location.  Depending on the output and options of the CAM systems, some manual editing of the program may be required. However, the overall changes will be minimal.

It is possible to create programs with angular start hole locations using “T” taper NC code or full 4-axis programs.  As part of all U/V axis machining, the taper data information (program plane, sub-plane, and Z-position) must be properly set and can be programmed using the G95 statement.

The images below show an example of a 15° angular hole in a workpiece with a height of 2.500 inches.  A tapered start hole is necessary because the top and bottom profiles do not intersect the Z-plane top View.  This example has been processed as a 4-Axis program, and the standard program NC code and modified NC code for the tapered start hole have been provided.   

Notable Replies

  1. We do each tapered hole as a single program using a different work coordinate system such as G55. Tip the wire as necessary and G92 the UV so the machine sees the UV as vertical. After running the part, switch back to G54 and return the UV to 0/0 and reset G55.

  2. Dan says:

    I alter the part geometry in MasterCam by the amount of the offset. That way I avoid offset errors in the machine control by not using G41 or G42.
    I loosely thread the wire thru the angled part start hole with UV at zero. My program has the angle of the start hole at the beginning with an M00 once angle is reached. To start the program, I turn the feed rate override knob down to 10% (Fanuc Alpha 1iC) Turn on dry run
    and press cycle start. UV axis move to the desired angle and stop. I turn off dry run. Gently tension the wire and start the program.
    For skim passes, I create separate programs for each pass with desired offset baked into the program. There is probably an easier way…
    But this works for me

Continue the discussion at Shop Talk >


Dynamic Filtration