[SOLVED:] Sketches get moved to another plane

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fr33cadtom
Posts: 12
Joined: Mon Jun 20, 2022 9:39 pm

[SOLVED:] Sketches get moved to another plane

Post by fr33cadtom »

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
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.
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bambuko
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Location: UK, England, North Devon

Re: Sketches get moved to another plane

Post by bambuko »

When I open your file in Master branch, I get following error messages:

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 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....
fillet face.png
fillet face.png (35.26 KiB) Viewed 2020 times


use Attachment editor to correct attachment mode:
In this case I used XY plane.
Good practice.
XY_plane.png
XY_plane.png (43.46 KiB) Viewed 2020 times


You can further offset the attachment to get it to the right place:
offset.png
offset.png (29.68 KiB) Viewed 2020 times


And the resulting model:
Screenshot from 2022-06-21 06.51.32.png
Screenshot from 2022-06-21 06.51.32.png (101.49 KiB) Viewed 2020 times

I didn't check anything else in the file - there may be other. similar problems...
modified file:
Ellen(bambuko).FCStd
(550.34 KiB) Downloaded 10 times
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
I am using Link branch and Assembly3
you can also download ... and try it here
excellent Assembly3 tutorials here
chrisb
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Re: Sketches get moved to another plane

Post by chrisb »

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.
You should retry with the now stable 0.20 version.
A Sketcher Lecture with in-depth information is available in English, auf Deutsch, en français, en español.
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bambuko
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Re: Sketches get moved to another plane

Post by bambuko »

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 :roll: :twisted: ;)
it was messing things up (and yes FreeCAD was hanging up as you have described)
Ellen(bambuko2).FCStd
(324.73 KiB) Downloaded 7 times
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 :ugeek: but that's another story
I am using Link branch and Assembly3
you can also download ... and try it here
excellent Assembly3 tutorials here
drmacro
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Re: Sketches get moved to another plane

Post by drmacro »

bambuko wrote: Tue Jun 21, 2022 7:09 am ...

What puzzles me is why it was so easy to solve it in Link branch and such a pain in Master branch :ugeek: but that's another story
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... 8-)
Star Trek II: The Wrath of Khan: Spock: "...His pattern indicates two-dimensional thinking."
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bambuko
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Re: Sketches get moved to another plane

Post by bambuko »

drmacro wrote: Tue Jun 21, 2022 10:14 am ...I'm not sure what you mean here....
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 :mrgreen:
I know what I like ;) (and so do you, I guess :lol: )
I am using Link branch and Assembly3
you can also download ... and try it here
excellent Assembly3 tutorials here
drmacro
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Re: Sketches get moved to another plane

Post by drmacro »

bambuko wrote: Tue Jun 21, 2022 10:37 am
drmacro wrote: Tue Jun 21, 2022 10:14 am ...I'm not sure what you mean here....
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 :mrgreen:
I know what I like ;) (and so do you, I guess :lol: )
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.

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."
fr33cadtom
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Re: Sketches get moved to another plane

Post by fr33cadtom »

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
drmacro
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Re: Sketches get moved to another plane

Post by drmacro »

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
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).

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."
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bambuko
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Re: Sketches get moved to another plane

Post by bambuko »

drmacro wrote: Tue Jun 21, 2022 2:15 pm .. then set the tip to the highest non-error feature and work my way down.
That's a good tip :lol: (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.
I am using Link branch and Assembly3
you can also download ... and try it here
excellent Assembly3 tutorials here
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