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Surface to solid

nyholkunyholku Member Posts: 58 PRO
Hi,

How do I turn a surface to solid?

I've got a 'cylindrical' surface created by sweeping an open arc along a closed path . . . how do I close the open ends and create a solid?

I guess I can close the open arc and sweep that to create a solid and then  boolean fill the centre but that feels like a hack ...


Best Answer

Answers

  • shanshanshanshan Member Posts: 147 ✭✭✭
    kustaa_2 ,hi,I think you can use "loft" feature to creat this solid,see the image below, the yellow lines are guide lines.

    loft.PNG 141.3K
  • nyholkunyholku Member Posts: 58 PRO
    Thanks, why did I not think about that, I will have a go!

  • nyholkunyholku Member Posts: 58 PRO
    Hmmm. Tried this but could not make it work. Loft as such would not let me select the top and bottom loops to loft between. I tried to create two sketches from the top and bottom and loft between them ... might have worked as it allowed me to select those but something went wrong and I did no persist as this seems about as much work as just filling the centre.
  • jakeramsleyjakeramsley Member, Moderator, Onshape Employees, Developers Posts: 621
    I would probably make a construction plane on the top and bottom to indicate the face.  Then I would thicken in all of the surfaces (they will be curved in based on the geometry you used).  To counter act the curvature, I would do a replace face of the top faces with the top construction plane and likewise with the bottom faces and the bottom construction plane.  Then I would delete all of the interior faces.

    1. Create construction planes on the top and bottom surfaces.  I used a plane point.


    2. Thicken the entire surface inwards a small amount.  Any small value should work.


    3. Replace the top four faces with the top construction plane.  Likewise with the bottom four faces with the bottom construction plane (this one will need to flip alignment as the top plane has a normal in the z-direction and the bottom faces have a normal in the negative z-direction).


    4. Delete the interior faces.




    The other option I was thinking was to make those same construction planes and then extrude a box that encompasses the surface up to those planes.  From here, you can split the part you just created and have the interior.

    1. Make a sketch of a rectangle that is larger than the desired part.


    2. Do a two directional extrude, both up to the surfaces that you created.


    3. Split the box with the surface you created.  Either delete or hide the unwanted part.



    Jake Ramsley

    Director of Quality Engineering & Release Manager              onshape.com
  • nyholkunyholku Member Posts: 58 PRO
    Ah, that seems like use trick to have in my bag and this does not feel like a hack, I like this approach. 

  • nyholkunyholku Member Posts: 58 PRO
    Just tried the box and cookie cutter method and this was easy, fast and intuitive now that I know about the split command. Thanks again.
  • andrew_troupandrew_troup Member, Mentor Posts: 1,584 ✭✭✭✭
    edited July 2015
    This is a good workaround for instances where the desired solid is bounded, in one direction, by extruded or revolved sketches (it seems to me).

    Planar surfaces, as we have top and bottom of this example, are equivalent to the simplest form of extruded sketch, where the sketch entity is a straight line.

    ON EDIT However, now that we have lofted surfaces, I see no reason why the method could not be bounded by these. And roll on other surface creation methods, including ruled surfaces, boundary surfaces and n-sided patches!
  • shanshanshanshan Member Posts: 147 ✭✭✭
    kustaa_2,kindly remind that maybe you do not know what you should notice when creating a loft feature. you should make each guide line connected with profiles,otherwise loft will show red in the loft dialog box, so see the two images below, can you notice any difference between them? in the first image, the guide line has a crossing point with the cirle center,but in the second image, the guide line has a crossing point with the circle,namely profile, so we just can creat a loft feature by lines in the second image successfully.I think using loft to creat your model is more direct!

  • shashank_aaryashashank_aarya Member Posts: 265 ✭✭✭
    @kustaa_2 Here is one more simple method I would like to suggest.

    Step-1 Apply thicken feature internally. Hide the surface. You can also delete it by delete feature.



    Step-2 Create datum planes by using three point option on both sides of the part for the three points as highlighted



    Step-3 Create the sketch on one of the newly created plane by projecting all the outer edges


    Step-4 Extrude the sketch up to bottom plane which is created by three point option.


    Result will be solid body as shown below.

  • 3dcad3dcad Member, OS Professional, Mentor Posts: 2,443 PRO
    Just an observation. I really hope this forum stays this way as time goes on - there is hardly ever unanswered questions and feeling of the forum is warm and very helpful towards new users. People across the world help each other to learn new tricks and I'm sure this forum will be quite a knowledge database for the people only following / searching for answers.
    //rami
  • nyholkunyholku Member Posts: 58 PRO
    Thanks everyone, real eye openers ... very useful answers ... so many ways to skin this cat! 

  • andrew_troupandrew_troup Member, Mentor Posts: 1,584 ✭✭✭✭
    edited July 2015
    @shashank_aarya
    It seems to me that (in the more general case) your method does require that the resulting body would need to be checked for hidden cavities.
    In some (but not all) cases these could be eliminated by increasing the dimension parameter of the thicken operation.
    In recalcitrant cases, it might not be possible to sufficiently increase the thickness without making an invalid body. However, it might be possible to use "Delete Face" if all the faces of each hidden cavity can be picked.
  • shashank_aaryashashank_aarya Member Posts: 265 ✭✭✭
    @andrew_troup Yes. I am agree with you. This method can be used when surface geometry is simple where thicken parameter can be increased sufficiently. For complex surfaces thicken may not work perfectly unless and until sufficient fillets are provided in surface. However we can try to thicken such surface with some workarounds like using multiple thicken options. But it may create non-uniform body on which we can add material by features like extrude, move face etc. This will ensure the availability of sufficient material while creating a final solid body as required.
  • chris_8chris_8 OS Professional Posts: 101 PRO
    Fantastic thread.  Using a surface to split parts is so simple, but I needed someone to point me to it.  Thanks jakeramsley!
  • frank_van_der_hulstfrank_van_der_hulst Member Posts: 3
    I have a similar issue, except I can't Thicken or otherwise the surface. I am trying to generate a model of a bee, and downloaded a SolidWorks model (search Public projects for "Bee.SLDPRT"). However, almost all the object is defined by surfaces rather than parts. The section I've started to look at is the abdomen, which is two surfaces which join down the centreline. Below is the right half.



    I really just want a "fill this volume" command!

    It seems that Thicken can't handle acute angles or something, because if I try to thicken the last tail piece it fails. I also tred Sketching a new object from the cross-section and revolving it, but then I get errors at the rounded end :( I did try Loft as well, but I'm not confident with that, and the edges on the surface go diagonally across it, so I don't think they're useful as guides.

    Any ideas?
  • jakeramsleyjakeramsley Member, Moderator, Onshape Employees, Developers Posts: 621
    I have a similar issue, except I can't Thicken or otherwise the surface. I am trying to generate a model of a bee, and downloaded a SolidWorks model (search Public projects for "Bee.SLDPRT"). However, almost all the object is defined by surfaces rather than parts. The section I've started to look at is the abdomen, which is two surfaces which join down the centreline. Below is the right half.



    I really just want a "fill this volume" command!

    It seems that Thicken can't handle acute angles or something, because if I try to thicken the last tail piece it fails. I also tred Sketching a new object from the cross-section and revolving it, but then I get errors at the rounded end :( I did try Loft as well, but I'm not confident with that, and the edges on the surface go diagonally across it, so I don't think they're useful as guides.

    Any ideas?
    https://cad.onshape.com/documents/7e2bffb436a244ff82095c80/w/2f849dd139a44950af8e7022/e/f13b188c83c64d01954fe8e5

    I made a volume encompassing it with an extrude then used the surface to split the solid.  This only works because the edges of the surface are planar.  I used a 3pt plane to create a sketch plane and then sketched a rectangle that is larger than the surface.  I then extruded it so that the edges of the surface touch the face of my extrude.  From here I used the split command to get a solid that has the boundary of the surface.
    Jake Ramsley

    Director of Quality Engineering & Release Manager              onshape.com
  • shanshanshanshan Member Posts: 147 ✭✭✭
    frank_van_der_hulst,please see the video below!

    3.gif 3.3M
  • andrew_troupandrew_troup Member, Mentor Posts: 1,584 ✭✭✭✭
    Well, I'll bee !   :)
  • frank_van_der_hulstfrank_van_der_hulst Member Posts: 3
    Brilliant! Many thanks!

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