Ticket #3436 - Fillet crash FC daily

[dbecad]

Good day,
I'm trying to reproduce a model seen in the forum (could not find original author for link), and finally got it to be fully parametric so that's good
As a final touch i was trying to apply fillet on some of the edges and some of them (see pict) just instant crash FC
Can anyone reproduce?
I search the topic and someone indicated to maybe refine the shape, but when i do that I cannot use the fillet from part-design WB.
Thanks for your help,
Cheers

fillet.png (26.65 KiB) Viewed 2052 times

---------------
OS: Ubuntu 16.04.4 LTS
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.18.13548 (Git)
Build type: None
Branch: master
Hash: 32973995423007a59cd18799c63383150811d1a7
Python version: 2.7.12
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 7.2.0
Locale: English/UnitedStates (en_US)

[chrisb]

I can confirm the crash and I have a solution for the fillet: Pad002 has a Refine property which you can set to True in the DataTab. Afterwards you can apply the fillet.

[dbecad]

Thanks Chrisb for the solution i'll keep that in mind if I encounter similar situation,
As follow-up
1/ should I open a tracker issue?
2/ Should body have a global refine option instead of individual features? (feature request?)

Thanks
Cheers

ping

[chrisb]

1/ should I open a tracker issue?
2/ Should body have a global refine option instead of individual features? (feature request?)

1/ Yes, the crash should be tracked. Please crossreference this discussion from the tracker and reply here with a link to the issue.

2/ There used to be a global solution controlled by preferences. This didn't work out, because models lost portability. You still can set the preferences to always use refinement, but I don't recommend it. I set it if necessary in a final step and if things don't work as expected - as in your case. The fact that the model was improved by refinement can not be generelized. So: no feature request required.

[HarryGeier]

it still can be set.. at least in .17 its still there.. and i have no Problems with it...

i hope the german screenshot is good enough.. its under tools->edit parameters

[chrisb]

You can still set it, it is in the Preferences editor as well, but the meaning has changed. In 0.16 the resulting model depended on the individual configuration prohibiting the exchange of models. This has completely changed, now it is only the default value to be set.

[dbecad]

Thanks ChrisB,
yeah I guess using refine on the last step if necessary kind of makes sense. First bug submitted
(hopefully i followed all rules )
Cheers

Trackback link:
https://www.freecadweb.org/tracker/view.php?id=3436

[Drest]

Hi,
I'm facing the same problem as dbecad with a file I'm working on.
I tried to refine the shape before adding the fillet, but Freecad still crash.

This is the fillet I'm trying to add :

filet.png (19.81 KiB) Viewed 1907 times

And the Freecad file I'm working on :

GoPro quick release casque sangles.fcstd

(802.74 KiB) Downloaded 37 times

I hope someone could help me to solve this problem
Drest

My Freecad infos :
OS: Ubuntu 18.04 LTS
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.17.13519 (Git)
Build type: None
Branch: releases/FreeCAD-0-17
Hash: 1a8b868018f45ea486c0023fdbfeb06febc1fb89
Python version: 2.7.15rc1
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 7.2.0
Locale: French/France (fr_FR)

[chrisb]

I hope someone could help me to solve this problem

A fillet cannot cross borders. Sketch009 is a problem: it makes the gap between the edge and the vertical offset arbitrary small, so that no fillet is possible. I would use an arc instead of a bspline and let it touch the other edge at an angle and not make it tangential.

Additionally there are some issues with sketches - besides the fact that you should always fully constrain them:
- You should rather use equality instead of repeating the same measure
- in Sketch007 you have a redundant vertical constraint, it is implied by the symmetry.
- The BSplines seem to generate problems if you want to reference in later steps external geometry. I will investigate this, but for now I would recommend to omit them.

[Drest]

Thank you chrisb, I'll try to modify my object and correct the sketches.
I'll come back here to tell if I succeeded
Drest.