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How to make a negative indentation from a 3d sketch?

Question asked by Paulo Esperon on Aug 6, 2017
Latest reply on Aug 6, 2017 by Paulo Esperon

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Hi there,

I have projected a sketch into a curved surface. Then I converted into a 3d sketch using convert entities. Now I would like to make a negative indentation (or a cut) in order to fit a part in the indent but for the life of me i cant do it.

If I want to cut extrude it asks me to select a direction and when I select it nothing happens.

I tried cutting from the top using the option to start cutting from the surface but I end up with an uneven indent (second picture)

Any ideas on how to go about this? I need the indentation to be the same depth all across.

Thank a bunch.

Paul Salvador Aug 6, 2017 3:49 PM

Correct Answer

..ok,.. I found out why.. .your revolve dome sketch is causing a singular or degenerative problem.. so... make the spline horizontal and the offset should now be clean... and, the Todd's first idea/suggest should work!... see attached image.

See the reply in context

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New Cast.SLDPRT.zip133.0 KB

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Todd Blacksher Aug 6, 2017 10:41 AM

I haven't looked at the file yet, but my first thought would be to use offset surface on the face created with your split line (with an offset of 0), use "Thicken" on the newly created surface, and then subtract it from the solid body using the "Combine" tool.

(Like I said, I haven't tried it, so I could be overlooking something, but this was what popped into my head.)

todd

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Paulo Esperon @ Todd Blacksher on Aug 7, 2017 8:04 AM

Hi Todd,

I just tried your approach but when I want to thicken the surface the tool does not allow me to do it. Any idea why?

It only works when I make it in the opposite direction of the body

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Paul Salvador Aug 6, 2017 3:32 PM

..I would totally agree with Todd Blacksher and without looking at it myself.. his suggestion should work!?

...although, this geometry had me thinking for some reason,... it seems too simple or am I missing something??

..I tried.. but,.. thicken cut, thicken and cut with surface does not play well with this spoke profile??

Why?... shaking head...

..so, for now,.. the workaround I did was extrude the spoke and thicken cut using the zero/offset inside surface.... then, combine/subtract.

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New Cast z.zip257.2 KB

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Paul Salvador @ Paul Salvador on Aug 6, 2017 3:49 PM

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Paulo Esperon @ Paul Salvador on Aug 7, 2017 8:04 AM

How remarkable that you found that detail. It works now!!

Thanks a lot Todd and Paul!

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5 Replies

Todd Blacksher Aug 6, 2017 10:41 AM
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I haven't looked at the file yet, but my first thought would be to use offset surface on the face created with your split line (with an offset of 0), use "Thicken" on the newly created surface, and then subtract it from the solid body using the "Combine" tool.
(Like I said, I haven't tried it, so I could be overlooking something, but this was what popped into my head.)
todd
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- Paulo Esperon @ Todd Blacksher on Aug 7, 2017 8:04 AM
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  Correct Answer
  Hi Todd,
  
  I just tried your approach but when I want to thicken the surface the tool does not allow me to do it. Any idea why?
  
  It only works when I make it in the opposite direction of the body
  Like • Show 1 Like1
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Paul Salvador Aug 6, 2017 3:32 PM
Mark Correct
Correct Answer
..I would totally agree with Todd Blacksher and without looking at it myself.. his suggestion should work!?
...although, this geometry had me thinking for some reason,... it seems too simple or am I missing something??
..I tried.. but,.. thicken cut, thicken and cut with surface does not play well with this spoke profile??
Why?... shaking head...
..so, for now,.. the workaround I did was extrude the spoke and thicken cut using the zero/offset inside surface.... then, combine/subtract.
Attachments
- New Cast z.zip257.2 KB
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- Paul Salvador @ Paul Salvador on Aug 6, 2017 3:49 PM
  Unmark Correct
  Correct Answer
  ..ok,.. I found out why.. .your revolve dome sketch is causing a singular or degenerative problem.. so... make the spline horizontal and the offset should now be clean... and, the Todd's first idea/suggest should work!... see attached image.
  Like • Show 3 Likes3
  Actions
  - Paulo Esperon @ Paul Salvador on Aug 7, 2017 8:04 AM
    Mark Correct
    Correct Answer
    How remarkable that you found that detail. It works now!!
    
    Thanks a lot Todd and Paul!
    Like • Show 2 Likes2
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How to make a negative indentation from a 3d sketch?

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