tooling marks on corner radius when profile milling
Close
Login to Your Account
Results 1 to 13 of 13
  1. #1
    Join Date
    Jul 2017
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    6
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default tooling marks on corner radius when profile milling

    Seems there is always a little tooling mark on the corners of parts I machine on Haas mills. I usually round corners with a .010" radius. It's only a couple lines of code around the radius, an IJK move. I do a finishing pass after roughing. I am using mastercam. I do not have the Haas HSM control option enabled.

    One way to eliminate this is to cut the parts with a square toolpath, then round the corners after, using slightly truncated corner radius geometry so that there is an angled lead into the cut. It would be more efficient not to have to do this however.

    Does anyone have other solutions?



  2. #2
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    1,474
    Post Thanks / Like
    Likes (Given)
    425
    Likes (Received)
    676

    Default

    I can't see your pics for some reason.
    I know others have had trouble posting pics when starting a thread.
    Could you repost them as a reply??

  3. #3
    Join Date
    Jul 2017
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    6
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

  4. #4
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    1,474
    Post Thanks / Like
    Likes (Given)
    425
    Likes (Received)
    676

    Default

    Obviously I don't know your complete application, but I'm not sure what the reason is for using I&J instead of R.
    For example approaching from X-3. with corner at 0,0.

    G1 X-.01
    G2 X0. Y-.01 R.01
    G1 Y-3.

    IDK if it makes a difference or not, but that's what I do to round off corners.

    Cheers.

  5. #5
    Join Date
    Jul 2017
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    6
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Thanks, I will try that. I'll need to change the default Haas machine controller settings in mastercam so that it codes arc moves differently.

  6. #6
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    951
    Post Thanks / Like
    Likes (Given)
    84
    Likes (Received)
    347

    Default

    how heavy is your finish pass? whats your IMP.
    what happens if you take a dry pass after your finish pass.

  7. #7
    Join Date
    Jul 2017
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    6
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    It seems, ChipSplitter, that the machine speaks IJK as fluently as it does radius.

    Good questions Delw. It probably IS an issue of cutter deflection, and, when the cutter rolls around the corner, it is effectively cutting at a much slower feed, the ratio between the centerline radius of the toolpath and that of the corner radius, which is .010", and the cutter is .5" diameter, a ratio of 1:25... so, a possible solution is to edit the corner radius feed rate to 25x that of the side wall to maintain a constant chip load. I only need to increase the feed rate to 1350 IPM around the corner! Problem solved. Well, the mini-mill feeds at a max rate of 500 so that will have to do. A 20IPM feed on the side walls and 500 at the corners would be a consistent chip load. Clearly, a smaller cutter is better suited to rolling fine corners. Cam's 2D high speed contour toolpaths do not seem to have a constant chip load feature.

  8. #8
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    1,474
    Post Thanks / Like
    Likes (Given)
    425
    Likes (Received)
    676

    Default

    Quote Originally Posted by prime_mover View Post
    It seems, ChipSplitter, that the machine speaks IJK as fluently as it does radius.

    Good questions Delw. It probably IS an issue of cutter deflection, and, when the cutter rolls around the corner, it is effectively cutting at a much slower feed, the ratio between the centerline radius of the toolpath and that of the corner radius, which is .010", and the cutter is .5" diameter, a ratio of 1:25... so, a possible solution is to edit the corner radius feed rate to 25x that of the side wall to maintain a constant chip load. I only need to increase the feed rate to 1350 IPM around the corner! Problem solved. Well, the mini-mill feeds at a max rate of 500 so that will have to do. A 20IPM feed on the side walls and 500 at the corners would be a consistent chip load. Clearly, a smaller cutter is better suited to rolling fine corners. Cam's 2D high speed contour toolpaths do not seem to have a constant chip load feature.
    The reason I use R is there is a lower chance of a rounding error and less math involved.
    IDK if it makes a difference or not, I just thought I'd throw it out there FWIW.

    If you don't have high speed machining turned on a Haas will struggle to maintain 100 ipm around a corner.
    It says its doing 500 ipm but it chokes up and slows down.
    Ask me how I know...

    What happens when you do a spring pass?
    Does the mark go away?

  9. #9
    Join Date
    Sep 2007
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    5,427
    Post Thanks / Like
    Likes (Given)
    225
    Likes (Received)
    1698

    Default

    Possibly the mark is due to your control looking ahead and dropping the feed rate to negotiate the corner. I can see the scallops in the straight section leading to the corner -- what feed rate was that? Seems like a decent feed rate, in which case the control might decide it needs to slow down to not violate the geometry at the corner. If the slowdown happens RFN instead of gradually, the cutter will dig in a bit.

    Regards.

    Mike

  10. #10
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    1,301
    Post Thanks / Like
    Likes (Given)
    862
    Likes (Received)
    1305

    Default

    Does it happen at every corner or just one? If just one corner. it could be the lead in/lead out of your profile.

  11. Likes toolsteel liked this post
  12. #11
    Join Date
    Nov 2012
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    2,134
    Post Thanks / Like
    Likes (Given)
    3500
    Likes (Received)
    2676

    Default

    I do not use Mastercam. But maybe this is similar. In Gibbs I would have an option of where to start and end that profile cut. Typically ppl start a profile cut off the part and then often times they will end the cut by wrapping around the 4th corner and ending at the tangent point where the corner rad meets the 1st side. Alot of times when actually running that tool path it will leave a mark where it ends due to tool deflection and since many of us are climb cutting that mark may actually be where the cutter got sucked into the material rather than being pushed away from the material. When that is the case taking a drift pass will maybe make it look slightly better but not eliminate it. Consider leaving more stock with a rough pass to allow for the cutter to get sucked in at the end of the rough pass but still leave material for finish pass to clean up entirely. If you want to check that theory....stop the machine between the rough and finish pass and blue up your part. Then run the finish pass only. You may see some blueing left after the finish pass which means you actually overcut it when roughing.
    If that doesnt solve it consider making 2 seperate tool paths with the foinish pass making a complete circuit around the profile but then continuing to run what was the first side of the part all the way off the end of the part.....in effect doing 5 sides.

  13. Likes Chris Attebery liked this post
  14. #12
    Join Date
    Jun 2002
    Location
    Gilroy, CA, USA
    Posts
    307
    Post Thanks / Like
    Likes (Given)
    215
    Likes (Received)
    19

    Default

    How much material are you leaving for the finish pass?

  15. #13
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    951
    Post Thanks / Like
    Likes (Given)
    84
    Likes (Received)
    347

    Default

    Quote Originally Posted by prime_mover View Post
    It seems, ChipSplitter, that the machine speaks IJK as fluently as it does radius.

    Good questions Delw. It probably IS an issue of cutter deflection, and, when the cutter rolls around the corner, it is effectively cutting at a much slower feed, the ratio between the centerline radius of the toolpath and that of the corner radius, which is .010", and the cutter is .5" diameter, a ratio of 1:25... so, a possible solution is to edit the corner radius feed rate to 25x that of the side wall to maintain a constant chip load. I only need to increase the feed rate to 1350 IPM around the corner! Problem solved. Well, the mini-mill feeds at a max rate of 500 so that will have to do. A 20IPM feed on the side walls and 500 at the corners would be a consistent chip load. Clearly, a smaller cutter is better suited to rolling fine corners. Cam's 2D high speed contour toolpaths do not seem to have a constant chip load feature.
    your getting too technical for a simple problem.

    What happens if you take a spring pass??
    boozebaily brings up another good point where is your start and finish? both should be completely off the part.


Tags for this Thread

Bookmarks

Posting Permissions

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