Part union fails

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geobruce
Posts: 33
Joined: Sat May 19, 2018 9:34 am

Part union fails

Postby geobruce » Sun Sep 16, 2018 7:27 pm

Hey

I get a infinitely long calculation time when trying to combine two parts.
* I checked the geometry and both parts are fine.
* I tried combine connected objects
* I tried UNION
* I tried UNION'ing them first with a cylinder through the parts
Nothing worked so far.

I would like to combine "ring1CutBot (Mirror #4)" with "ring1CutBot" and substract this as a whole from "ring body"

How should I do this?

you can find my file here: https://drive.google.com/open?id=1goWmo ... c5YNtWssZe

Thanks in advance
TheMarkster
Posts: 421
Joined: Thu Apr 05, 2018 1:53 am

Re: Part union fails

Postby TheMarkster » Mon Sep 17, 2018 1:25 am

I was able to make it work by deleting the mirror #4, changing the pad to 5.475mm, then cutting ring1cutbot out of the body, then mirroring that cut, and finally fusing the mirror with the cut.
helical gear.png
helical gear.png (24.92 KiB) Viewed 63 times
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NormandC
Posts: 16569
Joined: Sat Feb 06, 2010 9:52 pm
Location: Québec, Canada

Re: Part union fails

Postby NormandC » Mon Sep 17, 2018 1:50 am

Yeah, Boolean operations don't like co-planar faces between operators. It's always best when the objects being "Booleaned" intersect each other. In this case, Pad is the same thickness as ring1CutBot and its mirror combined. This can cause issues.

As for trying to fuse ring1CutBot and its mirror, no luck here either. A case of co-planar faces again, and the multiplied complexity is that they share a high number of edges.

TheMarkster wrote:
Mon Sep 17, 2018 1:25 am
changing the pad to 5.475mm
I raised the height of helix_sun1 by 0.1mm instead, this also succeeds even though one coplanarity condition remains (the bottom faces of ring body and ring1CutBot both still lie exactly on the global XY plane). The resulting Fusion of the Cut and its mirror checks OK with Part Check geometry.
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NormandC
Posts: 16569
Joined: Sat Feb 06, 2010 9:52 pm
Location: Québec, Canada

Re: Part union fails

Postby NormandC » Mon Sep 17, 2018 2:13 am

I was exploring an alternative that would have simplified the construction of the inner herringbone gear and possibly made it faster to compute. In the Part menu of the Part workbench, there is a Make face from wires command.

It is possible to create a parametric face from Ring1 outset and Sketch. Theoretically, you could then create a helical sweep from it, then mirror and fuse. Unfortunately, the resulting Sweep is invalid. Not sure why, as the face can be extruded without trouble. Maybe the face is created as B-spline instead of planar?
Attachments
helical gear face_simple_nc1.fcstd
(193.3 KiB) Not downloaded yet
FC_helical_gear_face_01.png
FC_helical_gear_face_01.png (33.86 KiB) Viewed 58 times
geobruce
Posts: 33
Joined: Sat May 19, 2018 9:34 am

Re: Part union fails

Postby geobruce » Mon Sep 17, 2018 5:02 pm

TheMarkster wrote:
Mon Sep 17, 2018 1:25 am
I was able to make it work by deleting the mirror #4, changing the pad to 5.475mm, then cutting ring1cutbot out of the body, then mirroring that cut, and finally fusing the mirror with the cut.

helical gear.png
thank you this helped me out