[SOLVED:] Sketches get moved to another plane
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- Posts: 12
- Joined: Mon Jun 20, 2022 9:39 pm
[SOLVED:] Sketches get moved to another plane
Here is my current version info:
OS: Windows 10 Version 2009
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.19.24267 +148 (Git)
Build type: Release
Branch: Branch_0.19.4
Hash: 476ecf091941bead59b14e44afa6064d5a66afa3
Python version: 3.8.6+
Qt version: 5.15.2
Coin version: 4.0.1
OCC version: 7.5.3
Locale: English/United States (en_US)
I have an issue where I have a sketch built on a face and when I reopen the file it ends up on another plane. I have tried to attach it to the correct face or to the xy plane, but then freecad hangs.
In the attached file it is the sketch called hubsketch.
I have had this issue with other files as well.
Any help would be appreciated.
thanks,
Tom
OS: Windows 10 Version 2009
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.19.24267 +148 (Git)
Build type: Release
Branch: Branch_0.19.4
Hash: 476ecf091941bead59b14e44afa6064d5a66afa3
Python version: 3.8.6+
Qt version: 5.15.2
Coin version: 4.0.1
OCC version: 7.5.3
Locale: English/United States (en_US)
I have an issue where I have a sketch built on a face and when I reopen the file it ends up on another plane. I have tried to attach it to the correct face or to the xy plane, but then freecad hangs.
In the attached file it is the sketch called hubsketch.
I have had this issue with other files as well.
Any help would be appreciated.
thanks,
Tom
- Attachments
-
- Ellen lamp gear-lg.FCStd
- (738.89 KiB) Downloaded 17 times
Last edited by fr33cadtom on Tue Jun 28, 2022 9:22 pm, edited 1 time in total.
Re: Sketches get moved to another plane
When I open your file in Master branch, I get following error messages:
I guess it is because I have no Gear workbench installed?
I am having difficulty getting it going in Master branch
so I opened it in Linkstage3 branch and...
Your sketch is attached to "fillet face"
Bad practice on many levels....
use Attachment editor to correct attachment mode:
In this case I used XY plane.
Good practice.
You can further offset the attachment to get it to the right place:
And the resulting model:
I didn't check anything else in the file - there may be other. similar problems...
modified file: I have used:
Code: Select all
07:45:45 <string>(1)<class 'ModuleNotFoundError'>: No module named 'freecad.gears'
07:45:45 <string>(1)<class 'ModuleNotFoundError'>: No module named 'pygears'
07:45:45 <string>(1)<class 'ModuleNotFoundError'>: No module named 'freecad.gears'
I am having difficulty getting it going in Master branch
so I opened it in Linkstage3 branch and...
Your sketch is attached to "fillet face"
Bad practice on many levels....
use Attachment editor to correct attachment mode:
In this case I used XY plane.
Good practice.
You can further offset the attachment to get it to the right place:
And the resulting model:
I didn't check anything else in the file - there may be other. similar problems...
modified file: I have used:
Code: Select all
OS: Ubuntu Core 20 (Pantheon/pantheon)
Word size of FreeCAD: 64-bit
Version: 0.21.29229 (Git) Snap 78
Build type: Release
Branch: master
Hash: 9db32a391142d9dbaf9e2d94c857a2a099e9d905
Python 3.8.10, Qt 5.15.3, Coin 4.0.0, Vtk 7.1.1, OCC 7.6.2
Locale: English/United Kingdom (en_GB)
Installed mods:
* DynamicData 2.46.0
* ToolViewReverse_ToolBar
* sheetmetal 0.2.49
* Manipulator 1.4.3
* Assembly3 0.11.3
* fasteners 0.3.40
* ThreadProfile 1.81.0
Re: Sketches get moved to another plane
You should retry with the now stable 0.20 version.fr33cadtom wrote: ↑Mon Jun 20, 2022 9:45 pm I have tried to attach it to the correct face or to the xy plane, but then freecad hangs.
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Re: Sketches get moved to another plane
I continued playing with it, and what solved it for me was deleting all the fillets, before re-attaching hubsketch to correct plane.
One of the fillets was corrupted with wrong edge and since your sketch was attached to the fillet
it was messing things up (and yes FreeCAD was hanging up as you have described)
File above is without fillets.
You can always add fillets as a last operation
What puzzles me is why it was so easy to solve it in Link branch and such a pain in Master branch but that's another story
One of the fillets was corrupted with wrong edge and since your sketch was attached to the fillet
it was messing things up (and yes FreeCAD was hanging up as you have described)
File above is without fillets.
You can always add fillets as a last operation
What puzzles me is why it was so easy to solve it in Link branch and such a pain in Master branch but that's another story
Re: Sketches get moved to another plane
I'm not sure what you mean here. I don't find fixing disenfranchised attachment difficult in master.
That is why I don't bother with linkstage3...
Star Trek II: The Wrath of Khan: Spock: "...His pattern indicates two-dimensional thinking."
Re: Sketches get moved to another plane
It wasn't criticism, just curiosity about the differences.
It is possibly to do with TPN differences?
i.e. in Master everything was crashing when I edited attachment (as described by OP) until I deleted offending fillets.
whereas in Link I just changed attachment and all was hunky-dory.
Not going to loose sleep over it
I know what I like (and so do you, I guess )
Re: Sketches get moved to another plane
My typical workflow in cases like this is to immediately set skip recomputes, then set the tip to the highest non-error feature and work my way down.bambuko wrote: ↑Tue Jun 21, 2022 10:37 amIt wasn't criticism, just curiosity about the differences.
It is possibly to do with TPN differences?
i.e. in Master everything was crashing when I edited attachment (as described by OP) until I deleted offending fillets.
whereas in Link I just changed attachment and all was hunky-dory.
Not going to loose sleep over it
I know what I like (and so do you, I guess )
Fillets are of course a bugger, since, by nature they depend on generated geometry.
Star Trek II: The Wrath of Khan: Spock: "...His pattern indicates two-dimensional thinking."
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- Posts: 12
- Joined: Mon Jun 20, 2022 9:39 pm
Re: Sketches get moved to another plane
All,
thank you for the suggestions and help. I have upgraded to version 0.20. I then deleted the fillets. When I originally created the hub sketch, I attached it to the face of the gear before I added the ring pad. I have no idea how it ended up being supported by the fillet but can see how that would be very bad.
I was able to support it on XY_Plane001. If I wanted to support it on the face of the gear, how would I do that? I tried several things but was unsuccessful.
Thanks again.
Tom
thank you for the suggestions and help. I have upgraded to version 0.20. I then deleted the fillets. When I originally created the hub sketch, I attached it to the face of the gear before I added the ring pad. I have no idea how it ended up being supported by the fillet but can see how that would be very bad.
I was able to support it on XY_Plane001. If I wanted to support it on the face of the gear, how would I do that? I tried several things but was unsuccessful.
Thanks again.
Tom
Re: Sketches get moved to another plane
Attaching to the face of the gear is not a good idea. That would be attaching to generated geometry and is like to result in what is called TNP. (Topological Namimg Problem).fr33cadtom wrote: ↑Tue Jun 21, 2022 10:43 pm All,
thank you for the suggestions and help. I have upgraded to version 0.20. I then deleted the fillets. When I originally created the hub sketch, I attached it to the face of the gear before I added the ring pad. I have no idea how it ended up being supported by the fillet but can see how that would be very bad.
I was able to support it on XY_Plane001. If I wanted to support it on the face of the gear, how would I do that? I tried several things but was unsuccessful.
Thanks again.
Tom
Which is quite likely what caused the issues to begin with. There were/are other sketches attached to generated geometry in the file I looked at.
Star Trek II: The Wrath of Khan: Spock: "...His pattern indicates two-dimensional thinking."
Re: Sketches get moved to another plane
That's a good tip (pardon the feeble pun)
I didn't think about it - probably because I practically never experience TPN TNP (it's so easy to avoid it )
so have little practice in recovering from the mess created by it...
Last edited by bambuko on Wed Jun 22, 2022 10:03 am, edited 1 time in total.