584,802 active members*
4,989 visitors online*
Register for free
Login
IndustryArena Forum > CAM Software > Mastercam > Mcam 9 3d surface help
Results 1 to 9 of 9
  1. #1
    Join Date
    Mar 2008
    Posts
    3

    Mcam 9 3d surface help

    Hello all,
    This is my first time posting here and I need some expert help. I am machining a pocket off an IGES file using a surface contour rought toolpath ( 3/4" roughter) and then a a surface finish with (3/8" ball mill) and I have some leftover I cannot remove using the leftover or pencil toolpaths on the bottom of the pocket. I am attatching some pictures as well. Thanks in advance for the help.
    Attached Thumbnails Attached Thumbnails rough.JPG   finish.JPG   problem w arrow.JPG  

  2. #2
    Join Date
    Apr 2003
    Posts
    3578
    Try using surface scallop instead to finish.
    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
    Cadcam
    Software and hardware sales, contract Programming and Consultant , Cad-Cam Instructor .

  3. #3
    Join Date
    Jul 2007
    Posts
    195
    You did not tell us what type of tool path you used so I can't tell you how to fix it.
    But try this, run a radial finish tool path. Set the angle settings to just cut the areas you need to clean up and use the center of the circle as the center of the tool path.
    Setup a boundry to keep the tool from bouncing off the finished wall and your done.
    Good luck
    Be carefull what you wish for, you might get it.

  4. #4
    Join Date
    Mar 2008
    Posts
    3
    I am running a surface finish Contour toolpath to finish the bump & machine radii. As far as setting the angle on a radial finish smooth toolpath, the problem area is on the bottom of the pocket so would I set a range of 0° to 0°? I have a circle drawn in to use as a boundary, but I have also have used the inside of the pocket as a check surface setting a 0.005 tolorace to stay off the walls, is this an incorrect way to do this? Thanks.

  5. #5
    Join Date
    Apr 2003
    Posts
    3578
    Finish contour is for profiling not for floors. to fix the floor use finish shallow.
    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
    Cadcam
    Software and hardware sales, contract Programming and Consultant , Cad-Cam Instructor .

  6. #6
    47,
    Draw a circle above the area to finish and use boundary with a scallop cut, this should clean that specific area. You can also use the boundary in shallow I believe.
    steve
    www.cad2cam.net
    www.cad2cam.net
    Programmer/ Certified Cam Instructor

  7. #7
    Join Date
    Mar 2008
    Posts
    3
    Thank you guys, I fixed it with your solutions!

  8. #8
    Join Date
    Dec 2005
    Posts
    15
    I have discovered this issue occur several times myself. Many times I have found you need to choose a smaller tolerance to reduce this scalloped remainder. Choosing a different toolpath function may work better also. The downside to these solutions is it often increases machining time significantly.

    One solution I have used often is to just create a surface patch around the problem area. Then add a surface cutting operation and simply pick off the remaining scallop.

  9. #9
    Join Date
    Apr 2003
    Posts
    3578
    One solution I have used often is to just create a surface patch around the problem area. Then add a surface cutting operation and simply pick off the remaining scallop.
    Why create a complex surface patch when you can define it with a simple arc or spline or rectangle and define this as a tool boundary with almost any surface toolpath.

    have found you need to choose a smaller tolerance to reduce this scalloped remainder.
    are you talking total tolerance ,example tighnting the surface tolerance ? or are you referencing the step over size as some people call this scallop tolerance.
    Just trying to better define what you are stating.
    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
    Cadcam
    Software and hardware sales, contract Programming and Consultant , Cad-Cam Instructor .

Similar Threads

  1. MCAM Lathe 101?
    By gearsoup in forum Mastercam
    Replies: 6
    Last Post: 06-30-2007, 02:48 PM
  2. Bummed about Mcam
    By cypher in forum Uncategorised CAM Discussion
    Replies: 14
    Last Post: 02-06-2006, 02:21 AM
  3. mcam??
    By tsutt in forum Mastercam
    Replies: 3
    Last Post: 09-26-2005, 06:03 PM
  4. MCam V8 and Fanuc 21 T
    By sleepless1 in forum Mastercam
    Replies: 7
    Last Post: 06-25-2005, 12:08 AM
  5. MCam 9.1 4th axis operation!! Please help.
    By deon in forum Mastercam
    Replies: 3
    Last Post: 03-13-2005, 11:20 AM

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •