Announcement

Collapse
No announcement yet.

3-D milling with BobCad

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

  • 3-D milling with BobCad

    Has anyone used BobCad to machine a part like this? I have
    BobCad V25 for milling but have never used it, long story.



    All I need to machine is the raised area on the one surface. How difficult is it to get BobCad to write a CNC program for this job?

    Thanks,
    Jim
    So much to learn, so little time

  • #2
    Perhaps posting this question on the Digital Thread here will yield more info ?

    http://bbs.homeshopmachinist.net/for...ital-Machinist

    Rich
    Green Bay, WI

    Comment


    • #3
      You can to do that with 2.5D, which BobCad should be able to do with little effort.

      Comment


      • #4
        I am curious as to what tool you would use to machine the two slanted faces? Assuming using CAM software and coming in with the tool perpendicular to the bottom flat face. Maybe a ball mill?
        Location: The Black Forest in Germany

        How to become a millionaire: Start out with 10 million and take up machining as a hobby!

        Comment


        • #5
          Originally posted by Black Forest View Post
          I am curious as to what tool you would use to machine the two slanted faces? Assuming using CAM software and coming in with the tool perpendicular to the bottom flat face. Maybe a ball mill?
          Ball end mill would be best, the bigger the ball, the larger the Z-step you can use without sacrificing the finish. If the radius between the flat and the feature is small, a end mill with a corner radius (bull nose) will work. Stepping down is fine for roughing, but for finishing with a ball end mill, going from the bottom up will give a better finish.
          George
          Traverse City, MI

          Comment


          • #6
            Danke!
            Location: The Black Forest in Germany

            How to become a millionaire: Start out with 10 million and take up machining as a hobby!

            Comment


            • #7
              Ball mill.. But it's a lot quicker to do a tool change and put a 45 degree face mill in and plow both sides (or just do it for "finishing" passes) . Better finish too.

              Comment


              • #8
                You certainly can do it with a ball end mill. But, you'll get a scalloped surface. Tilt the part and do the angled surface with a square end mill.

                Another way, if you have the tool, use a 45 degree tapered cutter.


                To the original question...quite easy to generate code in CAM. (Easy for me to say 'cause I do it all the time.)

                Comment


                • #9
                  Thanks for the replies. Originally I was thinking of using a 1/2" ball endmill. But now I think I can cut
                  the angles by simply tilting the workpiece in a vice. The workpiece is for a steel guitar and not particularly fussy. The piece is only 5" x 5" square.
                  Thanks,
                  Jim
                  So much to learn, so little time

                  Comment


                  • #10
                    Outback your part is finished. I cut it out of steel. Of course this is no help to you regarding BobCAM but it was an exercise for me.

                    I am trying Autodesk Fusion 360 and decided to model and setup the model in the cam and do a simulation of machining the part. I used a 10mm endmill and a 4mm ball endmill. One roughing pass with the ball endmill and then a finish pass. The finish pass is shown in brouwn.

                    http://youtu.be/fL6-Oa6aTjo
                    Last edited by Black Forest; 02-17-2015, 09:26 AM.
                    Location: The Black Forest in Germany

                    How to become a millionaire: Start out with 10 million and take up machining as a hobby!

                    Comment


                    • #11
                      Black Forest, in my earlier post about cutting from the bottom up with a ball end mill for better finish, that was for the finish pass only, cutting maybe .005"-.010" at most. The main shape is typically roughed out using larger bull nose or flat bottomed end mills from the top down.
                      George
                      Traverse City, MI

                      Comment


                      • #12
                        Originally posted by George Bulliss View Post
                        Black Forest, in my earlier post about cutting from the bottom up with a ball end mill for better finish, that was for the finish pass only, cutting maybe .005"-.010" at most. The main shape is typically roughed out using larger bull nose or flat bottomed end mills from the top down.
                        Now you tell me! Did you look at the video I posted?
                        Location: The Black Forest in Germany

                        How to become a millionaire: Start out with 10 million and take up machining as a hobby!

                        Comment


                        • #13
                          Just had a thought. If I supplied a Solidworks model of this part could someone here write the program?
                          My CNC mill runs on Mach3. This part will probably require some rounded edges not shown on the picture posted. I'm on vacation in Florida. The job was emailed to me from a regular customer. Don't have all the details right now but I know I'll get the job.

                          After 10 years of cnc machining this is the first job that requires 3D machining. I would hate to spend time and money learning BobCad for what could be a one time job.
                          Jim
                          So much to learn, so little time

                          Comment


                          • #14
                            Originally posted by Black Forest View Post
                            Now you tell me! Did you look at the video I posted?
                            Yes, saw the video and just looked again, see you changed it up a bit. Agree with others that tilting the part and cutting the angles that way is probably best for a one off part. My following comments are based on what I would do for a similar looking mold component in a commercial shop, where you always want to limit the setups. Machine time is cheap and you can be doing something else; flipping the part around takes money. Not saying this is the only way, or even the best way, it's just one way. Finish and size requirements might not call for as much monkey business. Of course, the home shop is a whole different ballgame...

                            Let's assume it's okay and desirable to leave a 1/8" radius at the base of the standing V. I would do a pocket (or clearing, or whatever your system calls it) toolpath with a large bull nose end mill, leaving about .010" stock on X and Y and on the Z flats. Either add the 1/8" rad to the model (best) or use a cutter with a nose radius of 1/8" or greater. Start at the top and don't get too wham jammy in your Z cuts; you don't want huge cusps interfering with the following cutters.

                            Once the part is roughed, finish the Z flats with a flat or bull nose end mill, keeping away from the radius. Run the pass a little high, check dimensions and run again to finish on size.

                            Next, I would run a semi finish program (ball end mill, same size as finisher) on the standing part and start at the top, leaving .002". After that, change to the finisher ball end mill and start at the bottom and step up, climb cutting.
                            George
                            Traverse City, MI

                            Comment

                            Working...
                            X