I get holes in a solid object after sweeping

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71GA
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Re: I get holes in a solid object after sweeping

Post by 71GA »

NormandC wrote:[One of these flaws is failed Boolean operations when one of the solid sits flush to a cylinder seam edge.
Could you explain this a bit more? I can't seem to interpret it. :)
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kkremitzki
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Re: I get holes in a solid object after sweeping

Post by kkremitzki »

71GA wrote:
NormandC wrote:[One of these flaws is failed Boolean operations when one of the solid sits flush to a cylinder seam edge.
Could you explain this a bit more? I can't seem to interpret it. :)
When you create a cylinder you have two circular faces for the top and bottom, and the central piece is sort of like a folded-up rectangle, glued to itself on a seam. You can see this seam in FreeCAD, and the seam edge is just the line segment that connects the top and bottom circular faces. If you have a solid that sits flush to this edge you can get unexpected Boolean operation failures.
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71GA
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Re: I get holes in a solid object after sweeping

Post by 71GA »

Thank you very much. So I guess until this is resolved in OCC I have to avoid using helix for making screws.
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bejant
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Re: I get holes in a solid object after sweeping

Post by bejant »

71GA wrote:So I guess until this is resolved in OCC I have to avoid using helix for making screws.
No, if you have problems just make sure that the helix doesn't start or end at the seam of the bolt blank.
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71GA
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Re: I get holes in a solid object after sweeping

Post by 71GA »

bejant wrote:No, if you have problems just make sure that the helix doesn't start or end at the seam of the bolt blank.
This doesn't work. I tried it like this and I still get empty space after I do a boolean cut...
Image
You can see that neither helix and neither swept profile are on the bolt seam...

The file:
Attachments
2017-03-27 -- outer threads -- v4.00.fcstd
(513.88 KiB) Downloaded 16 times
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NormandC
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Re: I get holes in a solid object after sweeping

Post by NormandC »

71GA wrote:This doesn't work. I tried it like this and I still get empty space after I do a boolean cut...
Apparently, this well-known workaround isn't working with the OCC version your FreeCAD version is compiled with (6.9.1).

Running Macro ForceRecompute on your model repairs it on the following FreeCAD version:

OS: Ubuntu 16.04.2 LTS
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.16.6707 (Git)
Build type: None
Branch: releases/FreeCAD-0-16
Hash: 5465bc47c95db45e0be85dc0e2872419efadce0f
Python version: 2.7.12
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 6.8.0.oce-0.17

Can you try with the AppImage available here: https://github.com/FreeCAD/FreeCAD/releases/tag/0.16

It is based on the Ubuntu package we provide in our PPA repo, and it's compiled with OCC 6.8.0.

I would also suggest another workaround that I've used in the past: remove the chamfer from the end of the screw (in Sketch); apply the cut between Pocket and Sweep; then create a new Revolution and use in a Part Cut on the bolt to make the chamfer.

EDIT: added file
2017-03-27 -- outer threads -- v4.00_normandc1.fcstd
(647.92 KiB) Downloaded 17 times
Apply a Cut between "Cut" and "Revolution001", the file exceeded the forum attachment limit if I apply it.
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