Announcement

Collapse
No announcement yet.

Simple questions about stock removal.

Collapse
X
 
  • Filter
  • Time
  • Show
Clear All
new posts

  • Simple questions about stock removal.

    Machinists,

    I'm just getting started running a cnc mill. Most of my experience is on a manual lathe. I've got a couple questions that should be easy for anyone who's done this.

    First, say you have a 3/4" deep object to mill the outside contour on, I put a piece of 1" stock in the machine and do my milling. Now how do I get the contour off the remaining 1/4" of material?

    Second, I need to mill a 2" round piece of stock into a smaller diameter (.75") 1/2" deep on the end. Easily done on a lathe, but how do you write the g-code to start making circles at 2" diam and end up at .75" diameter without writing a code for each circle? Or is that the only way. (This is the opposite of pocket milling)

    Thanks in advance,
    Jim

  • #2
    stock removal

    If you can securely hold what you just profiled, its not uncommon to flip the workpiece over and mill off the bottom.
    gvasale

    Comment


    • #3
      Jim,

      Each type machine control has a unique machine code.

      Some controls have conversational programing, and some strictly G and M
      function, and some a combination of both.

      You need to specify what machine, and control you have.

      With that info, I can write you a sample program provided we have a post processor for that control.

      You may still have to edit to make it run correctly.

      Best way is to get a manual from the manufacterer, or ebay, as a referance and learn to do it your self.

      If in business, there are cad-cam programs to assist you. Example Bobcad, or Mastercam. Lots of $$$.

      If it is a Bridgeport, I have a couple manuals I can send you.

      Kap

      Comment


      • #4
        Thanks, guys

        Im using Smithy 1034 cnc mill, Mach 3, Gecko drivers and steppers off a PMDX131 B.O.B..

        I'm learning g- and m- code and use the conversational often. Although it has pocket milling, it has not profiling like I need to do.

        If you have g-code for this type of application, I'd appreciate it.

        Regards,
        Jim

        Comment


        • #5
          Do you have a cam program? Check out Sheetcam.com. I use it and it is very good with excellent support and is constantly improving.

          Steve

          Comment


          • #6
            To cut the full profile of a part I often use double sticky tape to hold down the stock. For low profile parts tape works very well but you have to take lighter cuts than if the part was held mechanically.

            Make sure not to cut into the tape or you'll ball up the adhesive/chips and break the endmill. Leave .002" or so and file off the "flash" after removing the parts.

            Comment


            • #7
              I'll throw out another option for fixturing. If the part has thru holes, You can bolt it to a block of aluminium held in the vise. If the holes are clearance holes for a bolt, I'll drill the holes at nominal and then open them up to final size as a second op. You can either mill the profile a little deeper than the part into the aluminium block or stay above the block a few thousandths and then file off the remaining stock. I love this method because the profile will be square and all the features done at this time will be true to the profile.

              I've also mounted a piece on a aluminium block with toe clamps on the corners that will be waste (I had to turn a round piece out of fflat bar because we didn't have the right material) and milled the profile, leaving .010" which is enough to hold the part in place. Afterward a few whacks with a deablow breaks off the corners and the .010' left by the endmill and I cleaned it up with a file.

              Jon
              Jon Bohlander
              My PM Blog

              Comment


              • #8
                Assuming 2" circle, 1/2" tool, plunge down 1/2" goround once, move over and do goround to leave 0/75" boss.

                ;( T01 0.5 End Mill)
                N 20 G00 G20 G17 G90 G40 G49
                N 40 M05
                N 50 X0.0 Y0.0
                N 60 M06 T01
                N 70 M05
                N 80 Z1.9685
                N 90 M03
                N 100 S1000
                N 110 G04 P1.0
                N 120 F7.874
                N 130 X0.75
                N 140 Z0.1181
                N 150 G01 Z-0.5 F3.937
                N 160 G03 X0.75 I-0.75 J0.0 F7.874
                N 170 G01 X0.625
                N 180 G03 X0.625 I-0.625 J0.0
                N 190 G00 Z1.9685
                N 200 G28 Z0.0
                N 210 M30
                %

                .
                .

                Sir John , Earl of Bligeport & Sudspumpwater. MBE [ Motor Bike Engineer ] Nottingham England.



                Comment


                • #9
                  [QUOTE=
                  N 20 G00 G20 G17 G90 G40 G49
                  [/QUOTE]

                  John, not to quibble, but when I whent to programming school (GE Fanuc) we were taught to always right our code in assending order

                  G00 G17 G20 G40 G49 G80 G90 G98* for the safety line at the start of the program. Sure the control doesn't care but it makes it easier on the people who might have to edit later

                  * G98/99 Inch/Metric IIRC, its been awhile
                  Forty plus years and I still have ten toes, ten fingers and both eyes. I must be doing something right.

                  Comment


                  • #10
                    Originally posted by Spin Doctor
                    John, not to quibble, but when I whent to programming school (GE Fanuc) we were taught to always right our code in assending order

                    G00 G17 G20 G40 G49 G80 G90 G98* for the safety line at the start of the program. Sure the control doesn't care but it makes it easier on the people who might have to edit later

                    * G98/99 Inch/Metric IIRC, its been awhile
                    Spin,
                    Good point but to be honest that's what was in the post options and I have never bothered to notice it wasn't in ascending order.
                    G20 /21 is currently the option for inch / metric, was G70/71

                    G98/99 is currently Z level return after canned cycle but perhaps Fanuc is / was different.

                    .
                    .

                    Sir John , Earl of Bligeport & Sudspumpwater. MBE [ Motor Bike Engineer ] Nottingham England.



                    Comment


                    • #11
                      Thanks, John.

                      I'll try that.

                      Regards,
                      Jim

                      Comment

                      Working...
                      X