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How to create locking features on a split part?

going_alonggoing_along Member Posts: 9
I create a ring shaped part and split it in the plane of the rotation. Now I have two parts (A&B) with identical mating surfaces.

Next I want to create a torus shape (2 in fact one with slightly larger cross section) central and along the line of the original rotation.


Now add one of the torus shapes onto part A, subtract the other from part B to form a circular positional interlock between the parts, once 3D printed.

Sounds good but how do I go about it? I can create the elements but cannot seem to be able to select them for the Boolean operations. Is there a better way to achieve the same effect.

My apologies in case this question has already been asked but I did not know how to phrase search criteria for this condition.

Comments

  • owen_sparksowen_sparks Member, Developers Posts: 1,536 PRO
    Hi

    (Q1) It looks like you've made one torus a surface (in the revolve) rather than a solid.  Was that deliberate?  You'll not be able to boolean a surface to a solid.

    (Q2) Did you want the fit to be loose, or to snap into place?  If you're going for loose then you could add the torus to one part, and then boolean it away from the second with a small offset and eliminate the need for the second torus.

    Owen S.


    Production Engineer
    HWM-Water Ltd
  • larry_haweslarry_hawes Member Posts: 271 PRO
    edited June 13
    I wonder if you couldn't revolve 'remove' one ring and revolve 'add' the other to create the interlock you are looking for? Looks like you might need another sketch in the same location along the arc to perform the opposite operation (add versus remove)  I see you have sketch 3. See if the model below works for you...

    https://cad.onshape.com/documents/9797405c8d956c0cd65b7481/w/33629487f4030b9acfc9d77d/e/a07d7bb8263a2823b571c34d
  • Jake_RosenfeldJake_Rosenfeld Moderator, Onshape Employees, Developers Posts: 940
    @going_along

    Your approach seems fine, I think you are having trouble selecting for Boolean because the "larger ring" feature is set to "Surface" rather than "Solid".  You can see in the parts list that one of your rinds is a surface and one is a solid.  Once you go and change that, you can do one Boolean with "Union" and one with "Subtraction" as desired.

    Since the large parts obscure the rings, you can make the selection by either hiding the large parts, selecting from the parts list rather than the graphics area, or by using select other from the right click menu.
    Jake Rosenfeld - Modeling Team
  • larry_haweslarry_hawes Member Posts: 271 PRO
    edited June 13
    I tried the boolean operations but came no where near getting the operation completed. Converted to solids etc. but do not understand which, how, where to select parts etc. to achieve the result through boolean operations. Will try again. 

    Created a 'new' revolve instead of 'add' and that part was easily Boolean subtracted from Part 1 (or 2 can't remember).

    Seems a bit easier and straight forward to 'add' one revolve and 'remove' the other and skip boolean altogether but nice to see both methods. 
  • Jake_RosenfeldJake_Rosenfeld Moderator, Onshape Employees, Developers Posts: 940
    @larry_hawes

    You're right that it's easier to just use the "Add" and "Remove" options directly in the revolve.  I overlooked this in my answer.
    Jake Rosenfeld - Modeling Team
  • going_alonggoing_along Member Posts: 9
    Thank you everyone. I had not noticed that one torus was not solid as I had not deliberately selected for that. I tried recreating and even though I preselected for solid it came up as surface - is that due to the way I am selecting the part perhaps. Third time round it came up OK.

    As for the obscuration problem I have tried selecting from the parts list but it has never worked for me. I also tried using a sectional view but that did not seem to help either (meaning I could not select the torus I wanted even after suppressing the other). Finally achieved the selection I wanted but am not sure how.

    I feel that some clearance between the two torus is needed to allow for printed variation - hence having two. I like owen_sparks suggestion of using one but with an offset though I cannot see where that offset is introduced.


  • Jake_RosenfeldJake_Rosenfeld Moderator, Onshape Employees, Developers Posts: 940
    @going_along

    You'll notice that Boolean Subtract has an "Offset" option:


    You'll probably want to leave "Offset all" off and use the face of the torus as "faces to offset"
    Jake Rosenfeld - Modeling Team
  • larry_haweslarry_hawes Member Posts: 271 PRO
    Thank you everyone. I had not noticed that one torus was not solid as I had not deliberately selected for that. I tried recreating and even though I preselected for solid it came up as surface - is that due to the way I am selecting the part perhaps. Third time round it came up OK.

    As for the obscuration problem I have tried selecting from the parts list but it has never worked for me. I also tried using a sectional view but that did not seem to help either (meaning I could not select the torus I wanted even after suppressing the other). Finally achieved the selection I wanted but am not sure how.

    I feel that some clearance between the two torus is needed to allow for printed variation - hence having two. I like owen_sparks suggestion of using one but with an offset though I cannot see where that offset is introduced.


    In your original document I found that one of the tori revolves was 'added' and not 'new'. Since it was 'added' it could not be selected as a separate part as that did not create a 'new' part to perform the boolean operation. I could not select parts for the boolean operation either until that revolve was set to 'new'.
  • owen_sparksowen_sparks Member, Developers Posts: 1,536 PRO
    Hi all
    larry_hawes said:In your original document I found that one of the tori revolves was 'added' and not 'new'.
    Good catch Sir.
    Production Engineer
    HWM-Water Ltd
  • larry_haweslarry_hawes Member Posts: 271 PRO
    edited June 13
    Tried the offset operator in Boolean subtract and it worked a treat for this example - nice tip. As a side note, and something you most likely know you cannot do both Boolean Union and Boolean Subtract using the same part if you start with Boolean Union as there's no 'keep tool' option in the Boolean Union dbx. BTW who came up with 'Tool' to describe the Boolean operations? Very obscure and has fooled more than one you tube video user as well as myself as to its actual function and purpose.
  • going_alonggoing_along Member Posts: 9
    Again, thank you everyone. I got there finally.

    One thing I noticed was how quickly everyone saw the problems - and there was this from Jack_Rosenfeld "You can see in the parts list that one of your rinds is a surface and one is a solid." but I do not have a parts list view, just a Features List and it does not have that type of detail on it.

    You will have to excuse me I am just an electronics maker creating designs for school projects so I only come into 3D CAD when I need a new container or mechanical of some type.

  • Jake_RosenfeldJake_Rosenfeld Moderator, Onshape Employees, Developers Posts: 940
    Hi @going_along

    The parts list is at the bottom of the Feature List.  It may be hiding at the very bottom and need to be "slid up" by grabbing the bar above it.



    You may be interested in our "Onshape fundamentals" courses.  The first one goes over the user interface and points out all the little details like where to find the Parts List:
    https://learn.onshape.com/collections/onshape-fundamentals-cad

    If you still can't find the parts list, please post a screenshot of what you are seeing.  It's a big problem with our UI if it's not showing up!
    Jake Rosenfeld - Modeling Team
  • Jake_RosenfeldJake_Rosenfeld Moderator, Onshape Employees, Developers Posts: 940
    @larry_hawes

    If you do a revolve with "Add", you should be able to subtract the combined part from the other part with offset just fine (as long as you specify just the toroidal face as the face to offset).  There should be no need to keep the original tool around.  Here's an example:
    https://cad.onshape.com/documents/a984d23c132ec4ba23f27b3c/w/5be352b24d07178c6346e054/e/46d66dc736deae21a5bb175f
    Jake Rosenfeld - Modeling Team
  • larry_haweslarry_hawes Member Posts: 271 PRO
    @larry_hawes

    If you do a revolve with "Add", you should be able to subtract the combined part from the other part with offset just fine (as long as you specify just the toroidal face as the face to offset).  There should be no need to keep the original tool around.  Here's an example:
    https://cad.onshape.com/documents/a984d23c132ec4ba23f27b3c/w/5be352b24d07178c6346e054/e/46d66dc736deae21a5bb175f
    I like it - and mostly like the various methods to get the same thing accomplished.
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