Welcome to the Onshape forum! Ask questions and join in the discussions about everything Onshape.

First time visiting? Here are some places to start:
  1. Looking for a certain topic? Check out the categories filter or use Search (upper right).
  2. Need support? Ask a question to our Community Support category.
  3. Please submit support tickets for bugs but you can request improvements in the Product Feedback category.
  4. Be respectful, on topic and if you see a problem, Flag it.

If you would like to contact our Community Manager personally, feel free to send a private message or an email.

Has anyone ever done a Titan 9M in Onshape?

thomas_tabor
thomas_tabor Member Posts: 8 EDU
edited March 2021 in Community Support
Hey guys, working on my OnShape skills and hit a roadblock.  Working on the Titan 9M, and almost to the end, but at the pocket now, that has an angle in it and the pocket maintains a certain depth from the top plane.  Looking for some guidance.
Any help on how to accomplish the pocket and maintain the depth would be greatly appreciated.

Best Answer

  • thomas_tabor
    thomas_tabor Member Posts: 8 EDU
    Accepted Answer
    Thanks Steve, finally got it to work, I needed to change my plane, and then your settings work, AND now they make much more sense! 

Answers

  • steve_shubin
    steve_shubin Member Posts: 1,118 ✭✭✭✭
    @thomas_tabor

    If you could share the PDF of Titan 9M drawings, and also share the link to your document, I’m sure somebody could help


  • mahir
    mahir Member, Developers Posts: 1,324 ✭✭✭✭✭
    edited March 2021
    Did a little digging. Looks like the Titan-9M requires the pocket to be sketched from two directions. Here are a couple methods to do this.
    1. Create a solid with the proper shape using two orthogonal Extrude features. For example, extrude the top shape down, then cut away extra material from the side. Then, use a Boolean subtract to remove the material.
    2. Similarly, use two orthogonal Extrudes, but no Boolean. Instead, Cut using one extrude, then add material back with another extrude. On the second extrude you will likely need to extrude up to surface. This requires one less feature than #1, but it's probably less stable.
    In either case, save the fillets for last. Don't include them in your sketches.

  • thomas_tabor
    thomas_tabor Member Posts: 8 EDU
    I have attached the drawing. What I am struggling with is the .325 deep pocket that must follow the .325 depth from both the horizontal as well slanted surface.
  • steve_shubin
    steve_shubin Member Posts: 1,118 ✭✭✭✭
    edited March 2021
    @thomas_tabor

    Set extrude in the following way

    Solid
    Remove
    Up to part
    With an offset
    Make sure the offset is going in the proper direction
    And make sure that under Merge Scope, that your main part is selected

    The GIF takes 35 seconds to cycle.
    Make sure you watch the whole thing, in order to see all of the settings




  • thomas_tabor
    thomas_tabor Member Posts: 8 EDU
    Accepted Answer
    Thanks Steve, finally got it to work, I needed to change my plane, and then your settings work, AND now they make much more sense! 
  • NeilCooke
    NeilCooke Moderator, Onshape Employees Posts: 6,100 image
    Split face -> Move face -> Mic drop
    Senior Director, Technical Services, EMEA
  • steve_shubin
    steve_shubin Member Posts: 1,118 ✭✭✭✭
    edited March 2021
    @thomas_tabor

    Good to hear !


    @NeilCooke

    OK hold on a second before that mic drop

    Now I know I’m not the sharpest tool in the shed — FAR FAR FAR from it. LOL

    But it seems to me that this can’t be done with the move face/rotation, because the surface we're trying to end up with is conical

    But if there’s something I’m overlooking — which happens more often nowadays — let me in on it — I’d like to know what the secret is

    So in the GIF — the faces that I select, i.e. those highlighted in orange, those are conical surfaces



  • steve_shubin
    steve_shubin Member Posts: 1,118 ✭✭✭✭
    Made a rendering using V-Ray





  • NeilCooke
    NeilCooke Moderator, Onshape Employees Posts: 6,100 image
    @steve_shubin - your solution would make cleaner geometry and mine is no faster.
    Senior Director, Technical Services, EMEA
  • mahir
    mahir Member, Developers Posts: 1,324 ✭✭✭✭✭
    edited March 2021
    This would be pretty easy if Onshape had multi-thickness shelling. Vote for the improvement request!

Categories