[Solved]Cutout fails

[Rene]

Grabbed the v0.18 today and encountered an issue. Also tried already existing Sketch002 in the v0.17 and same result.

I put the Sketch002 to the YZ plane and want to make a Cutout (Through All and Reversed) = Pocket001 fails. If I use Dimension of 13,52mm it kinda works, but still not go through the wall.

Every other sketch and cutout I did after Sketch002 (for testing purposes) works as expected. Making this thread to know what I did wrong with Sketch002.

Is it something to do with the order I did things? The dependency graph looks weird, but that's all.

dep_001.jpg (82.41 KiB) Viewed 1687 times

OS: Windows 7
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.18.13971 (Git)
Build type: Release
Branch: master
Hash: 8e4dd8ca8496595d4718dc24c872f7ed668b2521
Python version: 2.7.14
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 7.2.0
Locale: Estonian/Estonia (et_EE)

[DeepSOIC]

Force recompute fixed the pocket for me. That suggests there might be a badly constrained sketch... further digging required...

UPDATE: Sketch001 reports a redundant constraint.

OS: Windows 10
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.18.13935 (Git)
Build type: Release
Branch: master
Hash: cb133767464337e4b5c8589a1fe33b4d7dad7721
Python version: 2.7.14
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 7.2.0
Locale: Russian/RussianFederation (ru_RU)

[chrisb]

In Sketch001 the vertical constraint to the right is implied by the symmetry. Remove it and recompute all.

[Rene]

Thanks for responses!
I fixed Sketch001, but it didn't fix the 4 holes. In the .gif I'm editing the Pocket001.

[chrisb]

Did you mark the root for recompute and recomputed all?

[Rene]

Yes, multiple times, but..

..I deleted the 4 holes and redid them. First they were just 4 random holes on the same plane and the pocket worked as expected. After I constrained the sketch more or less the same way I did originally - same fail. The issue is with my constraining! I guess I'll try 1 constraint at a time..

Edit: Sry, I didn't recompute the root! Will check my old file!

Edit2: Yes, I recomputed all the features, but not the root. It works perfectly now!

Thanks again!

[chrisb]

You're welcome. I would like to have a "Recompute all" button. It would mark the root and do the recompute in one step. This button could be like recompute but in red.

[NormandC]

The dependency graph looks weird

It looks perfectly fine. With the introduction of Part and Body containers, this is how it's supposed to look like. It does not look linear anymore.

[NormandC]

You did not attach Sketch001 correctly. It is unattached to anything, yet its Map Mode property indicates "FlatFace"; you set its Placement's Z value to 2mm. This is not the proper way in PartDesign now in v0.17.

You should attach Sketch001 to the Body's XY_Plane, then set its Attachment Offset Z property to 2mm.

[DeepSOIC]

Thanks for responses!
I fixed Sketch001, but it didn't fix the 4 holes. In the .gif I'm editing the Pocket001.

It's actually pretty strange. Makes me wonder, what exactly is messed up about shape previous to breaking pocket, that makes the pocket fail?... Bad constraints can cause problems while fusing/cutting coincident geometry, but in your case the cut that fails doesn't have any coincident geometry, just pure intersections.

Would be interesting if you find a step-by-step procedure to reproduce the problem from scratch.