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Need Better Modeling Strategy

robert_goldrichrobert_goldrich Member Posts: 4
I am trying to model a "roll-my-own" grid storage system, not unlike Gridfinity or others.


Illustration A shows the shape of my container -- except that it is solid, and I want a shell of that shape (i.e. by "imploding" the top face).  Illustration B shows the basic cross section, and C shows the error coming from the shell tool.  I'm sure this is not a bug from Onshape, but a problematic modeling strategy on my part.
Here is a link to the model in Onshape.  Any modeling tips will be greatly appreciated.  Many thanks in advance!  -Rob




Best Answers

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    john_lopez363john_lopez363 Member Posts: 103 ✭✭
    edited April 30 Answer ✓
    @robert_goldrich... not sure why but the problem is being caused by the "Chamfer".   Change your order of operation, add the Chamfers after the Shell.  And add the inside and outside Chamfers separately.
    EDIT:  You'll need to adjust the distance of inside Chamfer some (i used 2.5mm here).

    !


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    S1monS1mon Member Posts: 2,557 PRO
    Answer ✓
    There are many ways to solve this kind of issue. One would be to manually create the shell by offsetting the surfaces in two sets, and doing a mutual trim and then cutting out the inside with a split part. That would take a lot of face selections. The way I ended up doing it was to split the part (temporarily) into two parts, shell each of them, boolean union them back together, and removed a face so that you end up with a roughly constant wall.



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    wayne_sauderwayne_sauder Member, csevp Posts: 511 PRO
    Answer ✓
     As you can see there are many ways you could get this done. 
     In case you are still trying to figure out why that shell command doesn't work. Try reducing the wall thickness until it does. I think it is around .5 mm that it does work. This indicates that a thicker wall tries to create A. a wall thickness that is not uniform or B. a non-manifold geometry.   If you study these 2 subjects in depth the reason the shell tool gives an error makes some sense. I'm not quite sure what wall thickness you are going for but as is shown by the various examples there are ways to force this however there are 2 things that may show up non-uniform wall thickness and crazy things going on in the corners.  

     A couple of things that would make the shell command work.
     All corner fillets should have a radius larger than the wall thickness.
     The part that overhangs the chamfer needs to overhang by a dimension greater than the wall thickness. 

Answers

  • Options
    john_lopez363john_lopez363 Member Posts: 103 ✭✭
    edited April 30 Answer ✓
    @robert_goldrich... not sure why but the problem is being caused by the "Chamfer".   Change your order of operation, add the Chamfers after the Shell.  And add the inside and outside Chamfers separately.
    EDIT:  You'll need to adjust the distance of inside Chamfer some (i used 2.5mm here).

    !


  • Options
    S1monS1mon Member Posts: 2,557 PRO
    Answer ✓
    There are many ways to solve this kind of issue. One would be to manually create the shell by offsetting the surfaces in two sets, and doing a mutual trim and then cutting out the inside with a split part. That would take a lot of face selections. The way I ended up doing it was to split the part (temporarily) into two parts, shell each of them, boolean union them back together, and removed a face so that you end up with a roughly constant wall.



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    jnewth_onshapejnewth_onshape Member, Onshape Employees Posts: 72
    I have found modeling stacking structures is harder than it looks, particularly if they are molded. I noticed shell sometimes produces correct-but-weird results, as it does in your case. Looks ok, but you can see the steps and jogs and the weird corner condition at the internal filleted corners:



    The way I thought would be better is to explicitly define the wall profile, both inside and outside, via sketch. Then I perform a sweep for the wall and then add on a floor. I think the results look much better:



    Here's the doc: https://cad.onshape.com/documents/f4ee08d6980c2b0def0ee080/w/71443ae1dfc381b4bf6feb35/e/cb5fde0eca06ddd6c5ad5cb6

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    NeilCookeNeilCooke Moderator, Onshape Employees Posts: 5,524
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    wayne_sauderwayne_sauder Member, csevp Posts: 511 PRO
    Answer ✓
     As you can see there are many ways you could get this done. 
     In case you are still trying to figure out why that shell command doesn't work. Try reducing the wall thickness until it does. I think it is around .5 mm that it does work. This indicates that a thicker wall tries to create A. a wall thickness that is not uniform or B. a non-manifold geometry.   If you study these 2 subjects in depth the reason the shell tool gives an error makes some sense. I'm not quite sure what wall thickness you are going for but as is shown by the various examples there are ways to force this however there are 2 things that may show up non-uniform wall thickness and crazy things going on in the corners.  

     A couple of things that would make the shell command work.
     All corner fillets should have a radius larger than the wall thickness.
     The part that overhangs the chamfer needs to overhang by a dimension greater than the wall thickness. 
  • Options
    wayne_sauderwayne_sauder Member, csevp Posts: 511 PRO
     If you need any more examples.  :)
    https://cad.onshape.com/documents/ef11856685bcfc2a5bbbb116/w/8a7456388332f82135a94400/e/595474670b0b2df6b4d0bb12

    In the cell experiment, I used Neil's suggestion of a thin sweep. (Probably the best option.) 
    In the copy of the cell experiment, I got the shell command to work by increasing the size in Sketch 2 by a little (I realize this might not be an option, I am just showing what it takes to make it work). 

    If you allow me to, might I suggest that the grid be made in the same parts studio and be made to fit exactly by using an offset from the bin? 
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    S1monS1mon Member Posts: 2,557 PRO
    A thin sweep would have been nice, but the corner radii are not concentric.
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    robert_goldrichrobert_goldrich Member Posts: 4
    I want to express my sincere thanks to everyone who answered my query:  john_lopez363, Slmon, jnewth_onshape, robert_scott_jr_, NeilCooke, and wayne_saunder.

    I will need a day or two to digest this, but I so appreciate everyone taking the time to provide me with complete, competent, answers.

    I hope I get to pay it back or forward in the future!

    Rob

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    nick_papageorge073nick_papageorge073 Member, csevp Posts: 742 PRO
    S1mon said:
    A thin sweep would have been nice, but the corner radii are not concentric.
    I'm betting that was an oversight by @robert_goldrich. To Robert: for the radii to be concentric (they almost always should be), the outer one needs to be the inner radius plus the offset amount. 4.55mm in this case.
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