Mastercam WCS Origin
Close
Login to Your Account
Results 1 to 20 of 20
  1. #1
    Join Date
    Oct 2013
    Country
    UNITED STATES
    State/Province
    Arkansas
    Posts
    152
    Post Thanks / Like
    Likes (Given)
    48
    Likes (Received)
    13

    Default Mastercam WCS Origin

    I work for a carbon fiber bicycle company. Our VMC recently came back online after being down for some time, and I'd like to start machining molds on it. I've gone though several different CAM applications, and it's looking more and more like I'll be using Mastercam X5, which we already have. I learned Mastercam X7 in school years ago, but I'm struggling with something I don't think we worked with.

    Mold halves for any particular component on the frame are created with the origin maintained from the original bicycle skeleton sketch, so from each tool's perspective their origin would seem somewhat random. I need to make it so that if I click the top view, I am looking into the mold cavity with Y along the left side of the mold and X along the bottom. Currently the top view looks at a corner of the mold with the front as the left side and a different corner as the bottom.

    If I click WCS, then View Manager, then Solid Face..., it only allows me to select the Z. I need to define X and Y too, and neither are currently parallel or perpendicular to X and Y. I'm not sure where to go from here.

    Here's the top view currently:

    capture.jpg

    And the right view:

    capture1.jpg

    The top view is obviously wrong, and the right view shows the bottom.

    Can you walk me through changing these views?

  2. #2
    Join Date
    Feb 2006
    Location
    so cal, usa
    Posts
    504
    Post Thanks / Like
    Likes (Given)
    149
    Likes (Received)
    111

    Default

    In Mcam 2018, under transform, there's a command "move to origin" I'm sure such a command exists in your version of Mcam. Just click the top left corner ( or where ever you want the origin to be ) and you're in buisness.

  3. #3
    Join Date
    Oct 2013
    Country
    UNITED STATES
    State/Province
    Arkansas
    Posts
    152
    Post Thanks / Like
    Likes (Given)
    48
    Likes (Received)
    13

    Default

    Quote Originally Posted by greggv View Post
    In Mcam 2018, under transform, there's a command "move to origin" I'm sure such a command exists in your version of Mcam. Just click the top left corner ( or where ever you want the origin to be ) and you're in buisness.
    There is no corner. The chamfers are modeled.

    Is it possible to define X and Y by a side or an edge?
    Last edited by Veteran Bicycle; 01-30-2019 at 06:18 PM. Reason: Added X & Y question.

  4. #4
    Join Date
    Oct 2013
    Country
    UNITED STATES
    State/Province
    Arkansas
    Posts
    152
    Post Thanks / Like
    Likes (Given)
    48
    Likes (Received)
    13

    Default

    To be clear, the origin is unrelated to any of the geometry of the part, with perhaps the exception of what was the TOP plane when it was an .SLDPRT file in Solidworks. It appears to be the back view now, after exporting it as a STEP file and importing into MCAM X5.

    I am completely baffled how to associate the sides with right and front views. Totally lost. PLEASE HELP!

  5. #5
    Join Date
    Aug 2009
    Location
    Oakland, CA
    Posts
    302
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    126

    Default

    Just orient the part in a Solidworks assembly and import it to Mastercam from there.

  6. #6
    Join Date
    Oct 2013
    Country
    UNITED STATES
    State/Province
    Arkansas
    Posts
    152
    Post Thanks / Like
    Likes (Given)
    48
    Likes (Received)
    13

    Default

    Quote Originally Posted by TKassoc View Post
    Just orient the part in a Solidworks assembly and import it to Mastercam from there.
    I definitely tried that, but after a million tries I gave up.

    In fact I tried this from the beginning. I exported a STEP to a folder, then opened that STEP in Solidworks and did a move/copy feature. Despite trying every conceivable combination, it never opened in Mastercam in the correct orientation.

    Shouldn't this be simple? I just want to associate planar faces with WCS views! From what I see, my options are to pick the Z face and hope my X & Y line up. What if they don't?

  7. #7
    Join Date
    Oct 2013
    Country
    UNITED STATES
    State/Province
    Arkansas
    Posts
    152
    Post Thanks / Like
    Likes (Given)
    48
    Likes (Received)
    13

    Default

    I found a very good explanation on this page, but just like 100% of other posts I've found on the topic, there is no coverage of examples when I need to associate three sides to WCS views. It's always the Z and done.

    Easy going on Mastercam: WCS, T Plane & orienting the Part

  8. #8
    Join Date
    May 2005
    Location
    CA
    Posts
    1,058
    Post Thanks / Like
    Likes (Given)
    6
    Likes (Received)
    238

    Default

    Veteran Bicycle,

    I'm not sure this helps you, but will mention just in case.

    I use Fusion 360, and I model in it, and also do CAM in it. I can design something that is completely skewed in X/Y... with no relation to the global origin. When I switch to CAM, I have multiple choices on how to orient X/Y/Z, and can also select the origin either from "stock" box points or "model" box points (or actually can just be a point in space if I've drawn something in the design view that places a point "somewhere" which I can select).

    MasterCAM is surely as, or probably more capable than Fusion 360, so you should be able to orient X/Y/Z anywhere you want, and also make any point on stock, model, or otherwise... your origin.

    If it's any help, I can make a quick screen recording of how I do it, but ideally someone with MasterCAM will jump in and do that for you, which would be more relevant.

    PM

  9. #9
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    2,408
    Post Thanks / Like
    Likes (Given)
    1176
    Likes (Received)
    1182

    Default

    I am using X6, not sure if it is the same in X5. On the bottom toolbar you should see in the lower right some buttons, 3d/2d, Gview, Planes, WCS, level, etc. Click on the WCS button, select 'dynamic wcs', then select a corner of your part where you want your origin to be. From there, you can manipulate X Y Z axis however you like and drag them around, or enter an angle value. Note: This will create a new view in the plane manager, it does not actually move the part (which will be a good thing if you want to do any assembly type things), use this new view as your plane for machining and your toolpaths will be good to go.

  10. Likes Mtndew liked this post
  11. #10
    Join Date
    Jan 2014
    Location
    Temecula, Ca
    Posts
    2,462
    Post Thanks / Like
    Likes (Given)
    1129
    Likes (Received)
    3204

    Default

    I haven't used MC in a while, but from what I recall, you rotate the view the way you want it, then from the view manager you hit the "=" sign. That then becomes your top view.

  12. #11
    Join Date
    Oct 2013
    Country
    UNITED STATES
    State/Province
    Arkansas
    Posts
    152
    Post Thanks / Like
    Likes (Given)
    48
    Likes (Received)
    13

    Default

    Quote Originally Posted by Mike1974 View Post
    I am using X6, not sure if it is the same in X5. On the bottom toolbar you should see in the lower right some buttons, 3d/2d, Gview, Planes, WCS, level, etc. Click on the WCS button, select 'dynamic wcs', then select a corner of your part where you want your origin to be. From there, you can manipulate X Y Z axis however you like and drag them around, or enter an angle value. Note: This will create a new view in the plane manager, it does not actually move the part (which will be a good thing if you want to do any assembly type things), use this new view as your plane for machining and your toolpaths will be good to go.
    Thanks for the tip.

    There are no corners! The chamfers are modeled.

  13. #12
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    2,408
    Post Thanks / Like
    Likes (Given)
    1176
    Likes (Received)
    1182

    Default

    Quote Originally Posted by Veteran Bicycle View Post
    Thanks for the tip.

    There are no corners! The chamfers are modeled.

    Create a couple lines, use the trim function to extend one of them (or join both if you like), then select the corner. Or if you know where you want it, create a point and use that.

  14. Likes Mtndew liked this post
  15. #13
    Join Date
    Oct 2013
    Country
    UNITED STATES
    State/Province
    Arkansas
    Posts
    152
    Post Thanks / Like
    Likes (Given)
    48
    Likes (Received)
    13

    Default

    I added a coordinate system in Solidworks, and exported the STEP file including the coordinate system.

    Is there any way for Mastercam to respect that coordinate system when I open it?

    capture.jpg

  16. #14
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    4,275
    Post Thanks / Like
    Likes (Given)
    3782
    Likes (Received)
    2522

    Default

    Quote Originally Posted by Mike1974 View Post
    Create a couple lines, use the trim function to extend one of them (or join both if you like), then select the corner. Or if you know where you want it, create a point and use that.
    This is what you want to do, along with Mike1974's previous explanation.
    Translate Dynamic is the function you're looking for.

    OR
    Create a new plane, call it whatever you want, right click that plane,select edit,and move the datum to where you want, and also rotating it.
    It's very confusing at first, but once you see how it works it's really simple.

  17. Likes Veteran Bicycle liked this post
  18. #15
    Join Date
    Oct 2013
    Country
    UNITED STATES
    State/Province
    Arkansas
    Posts
    152
    Post Thanks / Like
    Likes (Given)
    48
    Likes (Received)
    13

    Default

    Quote Originally Posted by Mtndew View Post
    This is what you want to do, along with Mike1974's previous explanation.
    Translate Dynamic is the function you're looking for.

    OR
    Create a new plane, call it whatever you want, right click that plane,select edit,and move the datum to where you want, and also rotating it.
    It's very confusing at first, but once you see how it works it's really simple.
    I think I figured this out.

    I went back to the tooling master in Solidworks and removed the chamfers. Lesson learned.

    Then I used Dynamic WCS and had to manually rotate the axes to align with edges. I'm happy with the result.

    Thanks to all who have chimed in.

    capture.jpg

  19. Likes Mtndew, Mike1974 liked this post
  20. #16
    Join Date
    May 2005
    Location
    CA
    Posts
    1,058
    Post Thanks / Like
    Likes (Given)
    6
    Likes (Received)
    238

    Default

    VB,

    Not sure how others "model" parts, but I almost never model chamfers. In F360, they are much easier to program and cut if the corners are left sharp. Also, you may be able to just "suppress" the chamfer features in SW (rather than delete) and export your model with them turned off.

    PM

  21. Likes Mtndew liked this post
  22. #17
    Join Date
    Oct 2013
    Country
    UNITED STATES
    State/Province
    Arkansas
    Posts
    152
    Post Thanks / Like
    Likes (Given)
    48
    Likes (Received)
    13

    Default

    Quote Originally Posted by precisionmetal View Post
    VB,

    Not sure how others "model" parts, but I almost never model chamfers. In F360, they are much easier to program and cut if the corners are left sharp. Also, you may be able to just "suppress" the chamfer features in SW (rather than delete) and export your model with them turned off.

    PM
    Exactly what I did. Chamfers around the top edge are easy to program in HSM with a contour toolpath, but I've never figured out how to chamfer corners without having them modeled.

    I also changed my method slightly since posting above.

    I decided to draw a line coincident to the centers of the left and right edges, and use its centerpoint as the origin. This way I can keep my corners chamfered.

    Then I hide the line.

  23. #18
    Join Date
    Apr 2015
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    54
    Post Thanks / Like
    Likes (Given)
    4
    Likes (Received)
    4

    Default

    Also you don't necessarily need to sketch the new lines for the origin. If you drop the origin on one of the corners formed by the chamfered edges, align one axis along the edge adjacent, you can then drag it in a straight line along that oriented axis out into space and snap it to another edge and it'll align.

    For example, if you were trying to align to a lower left corner that was chamfered, you could drop the origin onto the 45 degree corner where the chamfer meets the edge you want to align with the X axis (horizontal edge). Then align X axis of the origin to that edge. Then grab the straight part of the arrow for the X axis and it allows you to drag it while maintaining the relations you just established. And it'll snap the origin in line with the edge you want to use for the Y axis.

  24. #19
    Join Date
    Apr 2006
    Location
    Ga.
    Posts
    128
    Post Thanks / Like
    Likes (Given)
    6
    Likes (Received)
    11

    Default

    Im pretty sure Solidworks front plane is Mastercam top plane.

  25. #20
    Join Date
    Feb 2019
    Country
    UNITED STATES
    State/Province
    Alabama
    Posts
    43
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    5

    Default

    In fact I tried this from the beginning. I exported a STEP to a folder, then opened that STEP in Solidworks and did a move/copy feature. Despite trying every conceivable combination, it never opened in Mastercam in the correct orientation.Shouldn't this be simple? I just want to associate planar faces with WCS views! From what I see, my options are to pick the Z face and hope my X & Y line up. What if they don't?


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
  •  
2