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.

Creating a plane "parallal" to a curved surface?

michael_fullermichael_fuller Member Posts: 23
So I need to extrude a detail into a curved surface, and in a perfect world that extrusion detail would be an offset of the host surface.  The only thing I can come up with for now is creating a plane that is offset from the surface in question, but the extrusion removal ends up being uneven, deep on one side, shallow on the other.  Is there a way to do this in OnShape?

Best Answer

Answers

  • _Ðave__Ðave_ Member, Developers Posts: 712 ✭✭✭✭
    Instead of extrude remove try extrude new and extrude to the curved face. You can now move offset the face the desired amount. Now just boolean subtract.  See vid below.



    2.gif 4.5M
  • philip_thomasphilip_thomas Member, Moderator, Onshape Employees, Developers Posts: 1,280
    This is an interesting one and a good teaching opportunity.
    The example below may or may not be what you're looking for - but everyone should find a nugget or two in the workflow :)




    Some of the nuggets;

    Splitting a body or face with a profile (Split1) - the trick here is to select the 'face' option
    Delete Face - this direct editing operation 'heals' the back side of this 'thing'.
    Move Face - (offset option) This creates walls that are perpendicular to the outside face. (note this cannot be molded)

    Have fun;

    https://cad.onshape.com/documents/4f75785542081efa7461dc57/w/a321fdf28bd5c33ee9b69480/e/48f228c936fbe13eddfeb391



    Philip Thomas - Onshape
  • _Ðave__Ðave_ Member, Developers Posts: 712 ✭✭✭✭
    Thanks @philip_thomas, great information there.
  • michael_fullermichael_fuller Member Posts: 23
    This is an interesting one and a good teaching opportunity.
    The example below may or may not be what you're looking for - but everyone should find a nugget or two in the workflow :)




    Some of the nuggets;

    Splitting a body or face with a profile (Split1) - the trick here is to select the 'face' option
    Delete Face - this direct editing operation 'heals' the back side of this 'thing'.
    Move Face - (offset option) This creates walls that are perpendicular to the outside face. (note this cannot be molded)

    Have fun;

    https://cad.onshape.com/documents/4f75785542081efa7461dc57/w/a321fdf28bd5c33ee9b69480/e/48f228c936fbe13eddfeb391





    This looks like it has potential.  However, when I go to delete faces, literally everything disappears and therefore there are then no faces to move.
  • michael_fullermichael_fuller Member Posts: 23
    I've gotten it to work.  Guess in the end I'm uncertain of the significance of the step where you "delete faces" as I've eliminated that step and it works regardless.
  • michael3424michael3424 Member Posts: 476 ✭✭✭
    Quick tip - if you are struggling with something - make the document public (and post the link here) and the people on this forum will fall over themselves to fix it for you. :)
    *And* explain how they fixed the problem, often with detailed graphics.
  • michael_fullermichael_fuller Member Posts: 23
    I've gotten it to work.  Guess in the end I'm uncertain of the significance of the step where you "delete faces" as I've eliminated that step and it works regardless.
    Michael - it will still work, but you will have the same split face on the back side.
    You could (for an interesting academic exercise);
    make a copy of the document for yourself
    mark the current state as a version
    branch from that newly created version
    suppress the 'delete face' feature in the new branch
    perform a 'compare' between the main branch and the new branch.
    the back side of the part will highlight showing the geometric difference.

    you might also equally, not do this. :)

    Quick tip - if you are struggling with something - make the document public (and post the link here) and the people on this forum will fall over themselves to fix it for you. :)

    OK, I understand making it public, how to do that.  I take it once I've made it public than everyone can see the URL once I paste it in?  Must admit I've been hesitant to do that, a paranoia about people stealing my work.  There is no hedge against that, is there?
  • philip_thomasphilip_thomas Member, Moderator, Onshape Employees, Developers Posts: 1,280
    @michael_fuller - Good question. 
    Many people post links to documents they have made public in order to get questions answered. 
    A public document may be copied by any user. Here are a couple of things you can do;
    1) Create a new document and construct a situation that is the same as your question, but does not disclose any proprietary information. You can do this in a number of ways; (a) not include the proprietary geometric details (b) copy/paste just the one part studio you have questions about (c) any number of other ways of obfuscating the proprietary information. Feel free to ask if you have more questions
    2) Create a new tab and move it to the front of the document and upload a pdf of bitmap describing the licensing terms under which you are making your document public - it could say simply "all rights reserved" or include at the other end, a full MIT license for example (this is the license under which we recently released our source code).

    Please consult a lawyer if you are planning on applying for a patent before any public disclosure.
    That said, that doesnt apply to 99% of the people here and most people freely post public links so that others can help them.

    Thank you for your support of Onshape.
    Philip Thomas - Onshape
  • dave_cowdendave_cowden Member, Developers Posts: 445 ✭✭✭
    Hi, I'm a little late to the party on this one, but I have created a featurescript Plugin that makes it easy to do what OP asked for-- create a plane tangent to a curved surface, and parallel with another one.

    You can get it free here:

    http://store.parametricparts.com/store/p2/PLANES-V1.0-BETA

    Enhanced planes lets you create planes in lots of ways, that makes this kind of problem easier.
Sign In or Register to comment.