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Loft - avoiding inner loops

salvatore_dianasalvatore_diana Member Posts: 5
Hi guys,

I'm trying to create a loft but I always get an error about "inner loops".I'm quite new to  cad so maybe there is a way to achieve what I want avoinding this problem.

I have a solid like this (it's something like a funnel), I've generated it with revolve:

What I want is that from the ring facing "Plane 1" in this image, it gradually becomes an ellipses, with the same thickness.
I've tried to:
1) Draw the same ring on a plane with offset 0 from the ring, and then two concentric ellipses in "Plane 1" but I incourred in "can't generate loft with inner loops inside"
2) Add a surface from the inner circle and the inner ellipses, and then thicken it. But the borders are not aligned:


Maybe I'm doing something wrong or there is a third better solution!
Can you help me?


Thanks!
Tagged:

Comments

  • owen_sparksowen_sparks Member, Developers Posts: 1,949 PRO
    edited April 2018
    Hi guys,

    ... and then two concentric ellipses...
    This is your problem.  You can have "nested profiles" on a loft sketch, ie one region within another.

    Fix (a) Use 2 sketches.  They can be on the same plane or surface.
    or
    Fix (b) Use i profile, loft as a solid, then use the shell command to hollow it out.

    Cheers,

    Owen S.

    Production Engineer
    HWM-Water Ltd
  • salvatore_dianasalvatore_diana Member Posts: 5
    Hi Owen,

    thanks for your answer! :)
    I didn't get what you mean with "Fix (a)"

    I tried to draw different sketches:


    I've drawn two sketches on face of Revolve 1 (inner and outer circle) and two sketches on Plane 1 (inner and outer ellipsis), but still can't manage to make it works.

    Can you give me further details on what you meant or anything to read/watch?


    Thanks! :)
  • owen_sparksowen_sparks Member, Developers Posts: 1,949 PRO
    Sure, in a meeting for half an hour or so. If nobody's jumped in after that I'll help.
    Production Engineer
    HWM-Water Ltd
  • owen_sparksowen_sparks Member, Developers Posts: 1,949 PRO
    Would you be happy posting a link to your doc?
    Production Engineer
    HWM-Water Ltd
  • billy2billy2 Member, OS Professional, Mentor, Developers Posts: 1,149 PRO
    @salvatore_diana ;

    one thing you might try is to work with surfaces. The last feature should be a thicken.

    Check this out, all surfaces:


    Do all your geometry created as surfaces, then thicken:


    Soon, you'll realize that solid modeling is a real pain. Trying to control the thickness of extruded solids is next to impossible. So, don't do that. Welcome to surface modeling! Build the outer skin of the organic shape, then at the end, just thicken it.

    Anyway, this is just another way to solve the problem. 




  • owen_sparksowen_sparks Member, Developers Posts: 1,949 PRO
    @salvatore_diana

    It looks like you got it to work :+1:  Is all good now?

    Cheers,

    Owen S.
    Production Engineer
    HWM-Water Ltd
  • salvatore_dianasalvatore_diana Member Posts: 5
    @owen_sparks:

    So, I created a new solid (loft) between outer circle and ellipsis, and then created another loft (remove) between inner circle and ellipsis.
    It works now! :)
    Is that what you meant in the first place?

    @billy2:

    Got your idea, but it seems quite unpraticable. Better to avoid this kind of approach as long as you can!
    Thank you anyway :)
  • Jake_RosenfeldJake_Rosenfeld Moderator, Onshape Employees, Developers Posts: 1,162
    @salvatore_diana

    Here is another workflow that may more closely resemble your original desired geometry:

    First, make an Loft that combines both the outer an inner profiles.  This will require that you hit the small triangle next to "Face of..." in the "Profiles" box and make profiles that have two selections:

    I've chosen to do an "Add" here because I thought that may match your design intent.

    Next, you'll want to do a "Remove" of a loft of the inner profile:



    Here's my copy of the document:
    https://cad.onshape.com/documents/690fb880f2a38887f17ce3f7/w/d92feb35590223be55e9a15d/e/bbd4a4915a7edc9a94e88ea5

    Feel free to use it in any way you see fit. 

    Hope this helps!
    Jake Rosenfeld - Modeling Team
  • Jake_RosenfeldJake_Rosenfeld Moderator, Onshape Employees, Developers Posts: 1,162
    Looks like I may have been too late :)

    Jake Rosenfeld - Modeling Team
  • salvatore_dianasalvatore_diana Member Posts: 5
    Looks like I may have been too late :)
    You have been helpful anyway! :smile:

    Thanks!
  • owen_sparksowen_sparks Member, Developers Posts: 1,949 PRO
    Brilliant minds think alike!
    Production Engineer
    HWM-Water Ltd
  • billy2billy2 Member, OS Professional, Mentor, Developers Posts: 1,149 PRO
    edited April 2018
    Surfacing is a different approach to modeling. I wouldn't do it for prismatic parts but hand held organic shapes I think they can benefit from this free form style. 

    So check this out:


    Adding Fill 2 completed the manifold (surfaces form nice edges & edges share common vertices). What's interesting is that OS changed the surfaces into a part without using "Enclose" feature. Well, this is definitely special functionality.

    So now that's it's a solid, shell it out:



    I think dealing with solids is more complicated. Each extrude has 4 to 6 surfaces that you're controlling and getting them all right is hard. With surfaces, I'm only dealing with one surface at a time and I feel I'm in control. At the end, solidify it and finish up the design.

    There's many ways to skin the cat! This is another one.

    Remember this one thing, there are no solids in solid modeling it's just a particular state of being for a bunch of surfaces.






  • Jake_RosenfeldJake_Rosenfeld Moderator, Onshape Employees, Developers Posts: 1,162
    Hi @billy2

    The designed behavior of "Fill" is that if you use "Add" and end up enclosing a region, it will convert to a solid.  If you think this behavior feels buggy, please file a feedback ticket or an IR.
    Jake Rosenfeld - Modeling Team
  • billy2billy2 Member, OS Professional, Mentor, Developers Posts: 1,149 PRO
    edited April 2018
    I guess I was more surprised than disappointed. Seems like I should take action to solidify knitted sheets.

    Or, maybe I should read the manual:


    So, how about this one:


    Loft using "Add" doesn't "Enclose":



    I suppose "Fill" is used to patch a hole in a manifold and therefore it should solidify once the manifold holds water.


    I like the "Fill" functionality, please leave it alone:

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