Hi,
I am trying to model a half circular edge / groove for a box. The model looks ok just before using the Additive pipe, but once the sweep is applied, the solid breaks. See the attached picture and model.
Here is the solid before the sweep:
Here is the sweep:
And once that Sweep (AdditivePipe) is applied, the top face disappears..
I am using the FreeCAD nightly build from Fedora copr: https://copr.fedorainfracloud.org/coprs ... d/nightly/
OS: Fedora 34 (Workstation Edition) (GNOME/gnome-xorg)
Word size of FreeCAD: 64-bit
Version: 0.20.pre_26154.fc34 (Git)
Build type: Unknown
Python version: 3.9.7
Qt version: 5.15.2
Coin version: 4.0.0a
OCC version: 7.5.0
Locale: Czech/Czech Republic (cs_CZ)
The same happens in the 0.19 stable AppImage:
OS: Fedora 34 (Workstation Edition) (GNOME/gnome-xorg)
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.19.24291 (Git) AppImage
Build type: Release
Branch: (HEAD detached at 0.19.2)
Hash: 7b5e18a0759de778b74d3a5c17eba9cb815035ac
Python version: 3.8.8
Qt version: 5.12.9
Coin version: 4.0.0
OCC version: 7.4.0
Locale: Czech/Czech Republic (cs_CZ)
[solved] Part design - Additive pipe - broken solid
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[solved] Part design - Additive pipe - broken solid
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Last edited by MarSik on Fri Oct 22, 2021 5:03 am, edited 1 time in total.
Re: Part design - Additive pipe - broken solid
Hi and welcome to the forum!
Your pipe has a self intersection at the right lower corner. That's one reason why you should always fully constrain your sketches: don't let anything be arbitrary.
Your pipe has a self intersection at the right lower corner. That's one reason why you should always fully constrain your sketches: don't let anything be arbitrary.
A Sketcher Lecture with in-depth information is available in English, auf Deutsch, en français, en español.
Re: Part design - Additive pipe - broken solid
Hi,
Thanks a lot. Fully constraining the sketches fixed the issue.
However, how did you find out? Is there any effective method of searching for problematic spots like this?
The sketch used to be fully constrained with sharp edges, but sweep did not like that. So I just used the Sketch workbench tool for fillets between two edges (CompCreateFillets) and that removed some of the constraints around the filleted corners (it would be nice if it could inherit those automatically...).
Best regardss
Martin
Thanks a lot. Fully constraining the sketches fixed the issue.
However, how did you find out? Is there any effective method of searching for problematic spots like this?
The sketch used to be fully constrained with sharp edges, but sweep did not like that. So I just used the Sketch workbench tool for fillets between two edges (CompCreateFillets) and that removed some of the constraints around the filleted corners (it would be nice if it could inherit those automatically...).
Best regardss
Martin
Re: Part design - Additive pipe - broken solid
Click on the triangle after the fillet tool, then you find there is a second fillet tool that preserves the constraints
Re: Part design - Additive pipe - broken solid
I know the movie "Casblanca" with the police chief's famous assignment "Arrest the usual suspects". And self intersections are such suspects.
A Sketcher Lecture with in-depth information is available in English, auf Deutsch, en français, en español.
- papyblaise
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Re: Part design - Additive pipe - broken solid
I agree whith Chris the bottom right R is too small =0.91mm , the mini is 1.01mm > the dia of edge is 2mm
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- Shalmeneser
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Re: Part design - Additive pipe - broken solid
(Too much useless DatumPlane.)
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Re: Part design - Additive pipe - broken solid
@Shalmeneser The Datum planes are not useless. They are used to mitigate the infamous Topology naming problem. This way no geometry depends on generated solids, it is all master sketch based. I could have probably offset the sketches themselves, but this way was easier to visualize and use in "Pad / Pocket until plane".
@papyblaise @chrisb - Thanks to both of you, I found it too after the first hint. I must have touched the overall geometry without realizing the unconstrained sweep path did not move (or in fact moved independently) properly.
Btw, I like the reference to Casablanca I remember that scene.
@papyblaise @chrisb - Thanks to both of you, I found it too after the first hint. I must have touched the overall geometry without realizing the unconstrained sweep path did not move (or in fact moved independently) properly.
Btw, I like the reference to Casablanca I remember that scene.
- Shalmeneser
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- Joined: Wed Dec 23, 2020 12:04 am
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Re: Part design - Additive pipe - broken solid
* I could have probably offset the sketches themselves : TRUE
* but this way was easier to visualize : TRUE
but you should create them just before using them. Your tree begins with 10 DatumPlane but it's difficult to know when they are used.
* .. and use in "Pad / Pocket until plane : OK, good remark
so you need the DatumPlane to be defined before.
When I do a pocket, I prefer to do it ThroughAll.