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Creating text on a concave surface

harry_blanekharry_blanek Member Posts: 5 ✭
in Community Support
I'm attempting to inscribe the word Kitty in a concave surface.  I first attempt to define an intersection line with the Plane that bisects the surface and it appears to be from top edge to top edge passing through the low point of the spherical section.  When I choose surface text I cannot seem to select the baseline I created with the intersection option but rather only half from top edge to lower center and the text shows up on one side or the other of the midpoint.  It seems it wants to use the arc I used to revolve the 'bowl' in the first place.  I've searched for surface text on a concave surface in help, on google and YouTube.  I've reviewed lots of videos about text on the outside of a sphere or ring but none that provide the epiphany of putting text where I want it in a hollowed out bowl.

I would either like to center the word 'Kitty' in the bottom of the circle or as an advanced idea, pick somewhere else on the surface and have the text go there.  I'm failing at all attempts.

Thanks in advance for suggestions.

Best Answers

  • matthew_stacymatthew_stacy Member Posts: 487 PRO
    Answer ✓
    @harry_blanek does this model accomplish the result that you are shooting for?  

    I changed your baseline sketch ("kitty intersection") with a single line segment, centered on the cavity.  That centering can be leveraged in the subsequent Surface Text feature.  Also note that made the sketch is now placed on a mate connector, aligned vertically, and tangent to that same cavity.  Also consider constraining (fully defining with dimensions and/or geometric constraints) your sketches.  Blue sketch elements indicate that there are remaining degrees of freedom to control. 



    Then in the Surface Text feature select the "centered" and "middle" options for text alignment.

     
  • jnewth_onshapejnewth_onshape Member, Onshape Employees Posts: 76
    edited June 10 Answer ✓
    @harry_blanek
    You have encountered a sort of funny bug in Onshape. The short version is that parasolid describes every location on a sphere's surface with two coordinates. At the very bottom of the basin (the way you drew it) that point is well-defined, but the vectors that describe a tangent face's orientation there are not, so custom features that rely on that tangent face tend to dislike it. I've filed a bug. 

    In terms of fixes: I ended up just drawing your circular cutout profile oriented differently, and then used "Text path" (which does more or less the same stuff as Surface Text just in slightly different fashion). That moves the "pole" of the sphere away from that center point where you want to write some letters. Then it just works:

    https://cad.onshape.com/documents/a1d4e1449a8c1af825345612/w/8c4b39db4b1fc7db2d031b97/e/328840af6461aeae739db432



    If you are interested you can read about "Text path" here: https://forum.onshape.com/discussion/comment/101716#Comment_101716 


Answers

  • _anton_anton Member, Onshape Employees Posts: 375
    If the surface is cylindrical, use the wrap feature. Else, Surface Text *should* be able to do it, possibly with some supporting geometry. Can you share a public link to the document?
  • harry_blanekharry_blanek Member Posts: 5 ✭
    edited June 9
    _anton, thank you for taking a look at my issue.   I can get text onto the surface of the hollowed out dish, but it doesn't center at the bottom.  The only baselines I am able to select in the Surface Text tool seem to be to the right or left of the point where the axis passes through the center of the drawing.  There is a baseline I created with the intersection command that appears to span the drawing from one side to the other.  I just can't seem to make the Surface Text command select that line.  

    https://cad.onshape.com/documents/c9f1ab6ffc9d4121e0661439/w/ab77db8baf0c7b9f4eb65dd0/e/7667d31524c5eca33e5619c3
  • matthew_stacymatthew_stacy Member Posts: 487 PRO
    Answer ✓
    @harry_blanek does this model accomplish the result that you are shooting for?  

    I changed your baseline sketch ("kitty intersection") with a single line segment, centered on the cavity.  That centering can be leveraged in the subsequent Surface Text feature.  Also note that made the sketch is now placed on a mate connector, aligned vertically, and tangent to that same cavity.  Also consider constraining (fully defining with dimensions and/or geometric constraints) your sketches.  Blue sketch elements indicate that there are remaining degrees of freedom to control. 



    Then in the Surface Text feature select the "centered" and "middle" options for text alignment.

     
  • jnewth_onshapejnewth_onshape Member, Onshape Employees Posts: 76
    edited June 10 Answer ✓
    @harry_blanek
    You have encountered a sort of funny bug in Onshape. The short version is that parasolid describes every location on a sphere's surface with two coordinates. At the very bottom of the basin (the way you drew it) that point is well-defined, but the vectors that describe a tangent face's orientation there are not, so custom features that rely on that tangent face tend to dislike it. I've filed a bug. 

    In terms of fixes: I ended up just drawing your circular cutout profile oriented differently, and then used "Text path" (which does more or less the same stuff as Surface Text just in slightly different fashion). That moves the "pole" of the sphere away from that center point where you want to write some letters. Then it just works:

    https://cad.onshape.com/documents/a1d4e1449a8c1af825345612/w/8c4b39db4b1fc7db2d031b97/e/328840af6461aeae739db432



    If you are interested you can read about "Text path" here: https://forum.onshape.com/discussion/comment/101716#Comment_101716 


  • harry_blanekharry_blanek Member Posts: 5 ✭
    @matthew_stacy and @jnewth_onshape, thank you much for your recommendations; your suggestions are great.  I've decided on a slightly different approach where I have a flat area on the bottom of the bowl/dish where I can have the text inscribed.  At least for now.  As an exceedingly CAD starter I am grateful for you taking the time to point me in a direction and advising things like set your dimensions...  Thank you much.
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