No announcement yet.

Most efficient way to mill small parts

  • Filter
  • Time
  • Show
Clear All
new posts

  • Most efficient way to mill small parts

    I recently cut some small parts on a Taig cnc mill(Max mill size is 3/16}I cut in layers using a 1/8 inch mill cutting 0.08 deep each pass editing Mach G code depth on each pass.What is the most efficient mill size to use and would cutting full depth with lower feed be better(Total thickness is 5/16 inch in mild carbon steel).I would like a small subroutine example to do this if layers are the best way to cut but I guess I don't quite understand the alteration of the code required. I also tried "Z" inhibit unsuccessfully.Thanks for any advice.

  • #2
    Get a free copy of CamBam plus. Andy has changed it so the Trial version will still allow you to create G-code up to a couple of hundred lines after the trial expires. It is turning into a really nice program and not just for G-code generation.

    Here is an example of a small part I just created in a couple of minutes. Note the parameters circled in red. They control the depth of cut, the cut ordering and the number of passes based on the bottom of cut final depth. It is all calculated automatically and I have rotated the part on the drawing area to show the layers of the tool path.

    Full disclosure: I was given a full version of the CamBam program for assistance in beta testing the program. I receive no other consideration.
    Free software for calculating bolt circles and similar: Click Here


    • #3
      As far as altering the g-code by hand, copy the block of code that cuts to a depth of .080". Paste the block after the one you copied and change the Z-0.08 value to Z-0.16 at each occurence of Z -0.08 in the second code block.

      Cut some air before trying it on a part.
      Free software for calculating bolt circles and similar: Click Here


      • #4
        Whats the top speed of the mill. That will best determine what size of end mill you can use.


        • #5
          Perhaps I am way off here, but I would make some manual cuts in the same material to get a feel for the various parameters. Start where you are with speed, DoC, feed rate, mill diameter, and then push each of the parameters and see the results. This is not a process that would guarantee the best result, but it will certainly get you further than you are now.

          Experiment with coolant too.
          Paul A.
          SE Texas

          Make it fit.
          You can't win and there IS a penalty for trying!


          • #6
            Since you are cutting steel, .08 DOC with a 1/8 e.m. is fine.

            To do the layers subroutine in G code, you would do something like this:

            (regular stuff like g code initialization, start up spindle, etc)

            (insert code to go to z-.08, e.g. ramp or spiral down)
            m98 p100 (runs subroutine)
            (insert code to go to z-.16)
            m98 p100
            (repeat as required)
            m5 m30 (end program)

            o100 (subroutine)
            (insert stuff here that describes the horizontal movement within an individual layer)
            (end-insert this comment here to make sure there is a line break after the m99)
            Last edited by beanbag; 06-12-2010, 05:24 PM.


            • #7
              I've looked at the subroutine thing a few times but where do you add the subroutine?Is it after the initial info like X,Y,Z,spindle speed and feed are entered or at the end of the first run so each run(loop) is a little deeper.I want to avoid editing the depth of Z for each run.Sorry for being dense about this.I


              • #8
                let's say that hypothetically you are going to machine a slot 3/16 inch wide and .25 inch deep and 2" long using a 1/8 end mill. Each "layer" is going to be .08 deep. You would have a single file that looks like this:

                (begin file)
                G0 G49 G40 G17 G80 G50 G90 G64 G20 (Inch)
                m3 s1600 (start up spindle)
                g0 x0 y0 z.1 (move to starting position)
                g1 z0 f1
                g1 z-.08 x.2 f3 (ramp down)
                m98 p100 (goto subroutine)
                g1 z-.16 x.2 (ramp down again)
                m98 p100
                g1 z-.24 x.2 (ramp down again)
                m98 p100
                g1 z-.25 x.2 (finishing pass)
                m98 p100
                g1 x.3 (cleans up remnant of ramp)
                g1 z.1
                g0 z1
                m5 m30 (stops spindle and main program)

                o100 (subroutine)
                g1 x2
                g1 y.062
                g1 x0
                g1 y0
                (end file)

                Any time the program sees m98 p100 it's automatically going to jump to the o100 part of the file, run that until it hits a m99, and then go back to the main body of the code where it left off.
                This program will run the 4 passes continuously without any input from you.