bug or incorrect use ? sketch breaks after changing a reference

[behn66]

Dear all,

kindly ask for help as I am facing similar issues quite often - and I am wondering if I just use the tool incorrectly or if it is indeed a bug I am encountering.
The issue with provided file is constant reproducable.

Description of the issue
-----------------------------------
I want to re-align a sketch, which is actually fixed horizontally by symmetry constraint.
So the old symmetry constraint gets deleted and to fully constrain the sketch again I am using "fix a point to object (shoft +o)" to re-align the sketch. However (hence this email) this "shift+o" move in y-axis in sketch breaks sketch003.
Still the same sketch, but horizontally moved.


How to reproduce
===================
1) load file

case-freecad.fcstd

(46.91 KiB) Downloaded 21 times

2) check sketch003, which just references two circles from sketch and remember the location of 3-circle and 4-circle
3) edit sketch:
- remove contraint 117 (symmetry) from sketch
- choose Element 26 (the circle) and choose the horizontal X-axis (going through 0/0) and choose "fix a point onto object (shift +o))
- sketch is now fully constrained, but has moved on y-axis
- here is the resulting file, see constraint 118 in sketch

case-freecad-modified.fcstd

(47.41 KiB) Downloaded 17 times

4) check again sketch003 - the two circles are now different ones. this is looking incorrect to me, hence this mail.


showing the change in sketch003 after modifying sketch
------------------------------------------------------------------------------------

sketch003.png (6.04 KiB) Viewed 1251 times

sketch003-changed.png (6.2 KiB) Viewed 1251 times

version used
=============
OS: Ubuntu 16.10
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.17.10460 (Git)
Build type: None
Branch: master
Hash: 91c59c7910436c44ede608e29d9a90a287121a11
Python version: 2.7.12+
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 7.1.0


Please let me know how to proceed here.

many thanks

christian

[DeepSOIC]

Hi, this is most likely issue #2721.

[DeepSOIC]

I just noticed you are using FC v0.17, so you can link to circles in the original sketch rather than to edges of solid. This will give you much more stable linking.

[behn66]

Dear DeepSOIC,

thanks alot. By looking into issue #2721 it sounds like a match.

I am not sure if I understood your proposal directly "link to circles in the original sketch rather than to edges of solid".
To do as you suggested, does it mean I shall choose Drawstyle->wireframe and then select the circle of the parent sketch as linked element?
Or how can I make sure to not use by accident an edge of a solid as link?

thanks

christian

[DeepSOIC]

To do as you suggested, does it mean I shall choose Drawstyle->wireframe and then select the circle of the parent sketch as linked element?

No. When editing Sketch003:
1. Switch to model tree, and hide all Pads/Pockets/whatever
2. Unhide the sketch you want to link to
3. and use external geometry tool to create the links

[behn66]

Dear DeepSOIC,

many thanks for making it clear to me - its now understood.

Many thanks

christian