Problem with Mastercam X6 flowline toolpath
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 28
  1. #1
    Join Date
    May 2009
    Country
    UNITED STATES
    State/Province
    Wyoming
    Posts
    2,795
    Post Thanks / Like
    Likes (Given)
    5993
    Likes (Received)
    4175

    Default Problem with Mastercam X6 flowline toolpath

    The cavity in the model is basically a funnel: a tapered extruded cut blending into a straight extruded cut with a fillet. For scale, the small end of the cavity is 3/8 inch radius. The radius of the fillet is 6 inches. Ideally, the surface of this cavity should be finished with continuous cuts end to end, which is supposedly the pattern of the "Flowline" finish toolpath. However, I absolutely can't get it to stop subdividing the toolpath into sections, which leaves facets and start/stop marks in the work.

    The response of the MC expert is, of course, that "There's something about the surface that Mastercam doesn't like, therefore the model must have surface errors" but I have verified that all sketch elements and surfaces are tangent and gap-free (those of you familiar with Solid Works know there's no way it will propagate a fillet across surfaces that cannot be made tangent, let alone a fillet that big). Anybody have any ideas about flowline; is there some parameter I am obviously overlooking? Appreciate any suggestions.


    orifice-block.jpg test-cavity-machined.jpg

  2. #2
    Join Date
    May 2017
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    163
    Post Thanks / Like
    Likes (Given)
    99
    Likes (Received)
    84

    Default

    I'd make edge curves on the solid and then make a fresh surface in Mastercam, ideally as all one piece.

  3. #3
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    3,447
    Post Thanks / Like
    Likes (Given)
    2807
    Likes (Received)
    1995

    Default

    Can you use the Morph between 2 Curves toolpath?

  4. #4
    Join Date
    May 2009
    Country
    UNITED STATES
    State/Province
    Wyoming
    Posts
    2,795
    Post Thanks / Like
    Likes (Given)
    5993
    Likes (Received)
    4175

    Default

    Quote Originally Posted by mhajicek View Post
    I'd make edge curves on the solid and then make a fresh surface in Mastercam, ideally as all one piece.
    Not sure I understand this. Do you mean remodel the part in Mastercam as opposed to importing the SW model?

  5. #5
    Join Date
    May 2009
    Country
    UNITED STATES
    State/Province
    Wyoming
    Posts
    2,795
    Post Thanks / Like
    Likes (Given)
    5993
    Likes (Received)
    4175

    Default

    Quote Originally Posted by Mtndew View Post
    Can you use the Morph between 2 Curves toolpath?
    Does X6 have this? What menu is it under?

  6. #6
    Join Date
    May 2009
    Country
    UNITED STATES
    State/Province
    Wyoming
    Posts
    2,795
    Post Thanks / Like
    Likes (Given)
    5993
    Likes (Received)
    4175

    Default

    I should've mentioned, roughing the cavity was not a problem, we used Surface High Speed Scallop which works well.

    The Mastercam guy just sent me his recommended finish method: Surface finish contour stepping down in Z, followed by Surface Finish Parallel at 90 degrees to the previous paths.

    Apparently Flowline is intended for single surfaces. It has an inherent inability to deal with multiple surfaces. If I understood it correctly, Mastercam's internal computation produces tiny mismatches, which it then interprets as surface deviations. Kind of a Catch-22, especially when you have been looking at those beautiful full-color screenshots in their magazine ads. Oh, well; hellloooo cycle time...

    Thanks for the replies, BTW

  7. #7
    Join Date
    Sep 2007
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    4,464
    Post Thanks / Like
    Likes (Given)
    82
    Likes (Received)
    1004

    Default

    Quote Originally Posted by Oldwrench View Post
    Apparently Flowline is intended for single surfaces. It has an inherent inability to deal with multiple surfaces. If I understood it correctly, Mastercam's internal computation produces tiny mismatches, which it then interprets as surface deviations. Kind of a Catch-22, especially when you have been looking at those beautiful full-color screenshots in their magazine ads. Oh, well; hellloooo cycle time..
    I have a part programmed in MCAM 2017 that Flowlines across 3 subtlely sloped surfaces, so it can be done. If there were any mismatches, I'd see them in the code and the resulting surfaces, but the surfaces flow very smoothly into each other.

    Regards.

    Mike

  8. #8
    Join Date
    May 2017
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    163
    Post Thanks / Like
    Likes (Given)
    99
    Likes (Received)
    84

    Default

    Quote Originally Posted by Oldwrench View Post
    Not sure I understand this. Do you mean remodel the part in Mastercam as opposed to importing the SW model?
    I mean to remodel just that surface / those surfaces. Should be really quick and easy. If it's multiple surfaces, try checking the "single row only" box on the third tab of the flowline operation's parameters.

  9. #9
    Join Date
    May 2009
    Country
    UNITED STATES
    State/Province
    Wyoming
    Posts
    2,795
    Post Thanks / Like
    Likes (Given)
    5993
    Likes (Received)
    4175

    Default

    Quote Originally Posted by Finegrain View Post
    I have a part programmed in MCAM 2017 that Flowlines across 3 subtlely sloped surfaces, so it can be done. If there were any mismatches, I'd see them in the code and the resulting surfaces, but the surfaces flow very smoothly into each other.
    Well, these flow very smoothly into each other too, onscreen. Onscreen it's flawless!

    Further discussion with the MC tech has revealed that flowline will handle sloped intersecting surfaces as long as they are relatively flat; where it breaks down is intersecting curved surfaces, particularly those where the cut lines would converge. Apparently MC will not allow cut lines to be superimposed and it will force a minute jog to avoid it—even if, as in this case, it would improve the finished surface to have them do so.

    I have eliminated the machine itself as a source of the problem; running the toolpath at 90° in another test part reproduces the facets exactly. This has been an interesting exercise but it's time to make the parts. I came up with a workaround that should minimize the hiccups. We shall see (said the blind man, as he picked up his hammer and saw).

    If it gets the parts close enough to stone, I know how to do that.

  10. #10
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    3,447
    Post Thanks / Like
    Likes (Given)
    2807
    Likes (Received)
    1995

    Default

    Quote Originally Posted by Oldwrench View Post
    Does X6 have this? What menu is it under?
    It's a multiaxis toolpath,but can be posted for 3,4, and 5 axis machines

  11. #11
    Join Date
    Dec 2008
    Location
    tempe,arizona,usa
    Posts
    1,586
    Post Thanks / Like
    Likes (Given)
    127
    Likes (Received)
    174

    Default

    So did you create the SolidWorks part?

    if so you could have build that face to not have the breaks in it, that way it would be one segment instead of 3. I am assuming it is a lofted cut....?

    put up the SW model an I'll show you how.

  12. #12
    Join Date
    May 2009
    Country
    UNITED STATES
    State/Province
    Wyoming
    Posts
    2,795
    Post Thanks / Like
    Likes (Given)
    5993
    Likes (Received)
    4175

    Default

    Quote Originally Posted by len_1962 View Post
    So did you create the SolidWorks part?

    if so you could have build that face to not have the breaks in it, that way it would be one segment instead of 3. I am assuming it is a lofted cut....?

    put up the SW model an I'll show you how.
    No, it's not a lofted cut, it's two simple extruded cuts. One has draft, the other is straight. They intersect on a common axis. The intersection is filleted. Thanks for offering to show me how to make the die differently, but its design is highly specific to its purpose and not subject to change. Anyway, having designed all this company's products in SW since 2001 I can assure you the issue isn't with the model, it's with the limitations inherent in Flowline. But thank you for the thought.

  13. #13
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    3,447
    Post Thanks / Like
    Likes (Given)
    2807
    Likes (Received)
    1995

    Default

    Quote Originally Posted by Oldwrench View Post
    No, it's not a lofted cut, it's two simple extruded cuts. One has draft, the other is straight. They intersect on a common axis. The intersection is filleted. Thanks for offering to show me how to make the die differently, but its design is highly specific to its purpose and not subject to change. Anyway, having designed all this company's products in SW since 2001 I can assure you the issue isn't with the model, it's with the limitations inherent in Flowline. But thank you for the thought.
    Would a loft surface be different/change the surface tolerances? I don't have much experience with creating surfaces, but flowline would handle it better if it were 1 complete surface.
    Another option would be to use a parallel toolpath.

  14. #14
    Join Date
    Jun 2013
    Country
    UNITED STATES
    State/Province
    California
    Posts
    901
    Post Thanks / Like
    Likes (Given)
    610
    Likes (Received)
    404

    Default

    Just use Surface Finish Scallop
    done deal!!

    Surface Finish blend might be decent, but won't beat scallop, IMHO.

  15. Likes mhajicek liked this post
  16. #15
    Join Date
    Jun 2013
    Country
    UNITED STATES
    State/Province
    California
    Posts
    901
    Post Thanks / Like
    Likes (Given)
    610
    Likes (Received)
    404

    Default

    Quote Originally Posted by Oldwrench View Post
    Anybody have any ideas about flowline; is there some parameter I am obviously overlooking? Appreciate any suggestions.

    Flowline originated in MC as a single surface-patch toolpath. It has been improved over the years to include multi surfaces, but you're seeing the limitation.

  17. Likes Oldwrench liked this post
  18. #16
    Join Date
    May 2009
    Country
    UNITED STATES
    State/Province
    Wyoming
    Posts
    2,795
    Post Thanks / Like
    Likes (Given)
    5993
    Likes (Received)
    4175

    Default

    Quote Originally Posted by Mtndew View Post
    ...flowline would handle it better if it were 1 complete surface.
    Another option would be to use a parallel toolpath.
    I have learned that Flowline requires that the complete surface not deviate too far from a common plane. The problem is especially acute with tapered holes. It doesn't care whether it's constructed via a drafted cut-extrude or via lofting. It also doesn't matter if the surface is error-free all the way to the computational limit of SW, which is a lot of decimal places. When individual cut lines converge to the point of intersecting, Mastercam will force a small jog and that is the obstacle with this particular shape. I'm on X6 but the flowline toolpath in MC2017 won't do it either. Likewise, any parallel toolpath necessarily has jogs when executing a tapered hole, which means it will rough but not finish in the lengthwise direction.

    We are getting around it by doing Finish Flowline in narrow sections, which it seems to allow. The die sets are all similar to this example except that the diameter of the small end varies. Machining time is under an hour each in S7 tool steel and I can hand-blend them in about 10 minutes. Problem solved...or at least as well as it needs to be in this case. Thank you all who contributed.

  19. Likes Mtndew liked this post
  20. #17
    Join Date
    Jun 2013
    Country
    UNITED STATES
    State/Province
    California
    Posts
    901
    Post Thanks / Like
    Likes (Given)
    610
    Likes (Received)
    404

    Default

    Parallel is No bueno, IMO, because there will be huge step downs on vertical walls and nice small step overs on horizontal.

  21. Likes Mtndew liked this post
  22. #18
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    3,447
    Post Thanks / Like
    Likes (Given)
    2807
    Likes (Received)
    1995

    Default

    Quote Originally Posted by mkd View Post
    Parallel is No bueno, IMO, because there will be huge step downs on vertical walls and nice small step overs on horizontal.
    Yeah, I don't use Parallel that much. Flowline is usually my go-to.

  23. #19
    Join Date
    Sep 2013
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    131
    Post Thanks / Like
    Likes (Given)
    7
    Likes (Received)
    24

    Default

    Does MC X6 have the hybrid path which is a combo z-level and floor contour? I don't recall what the name of it is.

  24. #20
    Join Date
    Jun 2013
    Country
    UNITED STATES
    State/Province
    California
    Posts
    901
    Post Thanks / Like
    Likes (Given)
    610
    Likes (Received)
    404

    Default

    Quote Originally Posted by Qwan View Post
    Does MC X6 have the hybrid path which is a combo z-level and floor contour? I don't recall what the name of it is.
    _called Hybrid in the High speed menu LOL


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
  •