Sheet Metal workbench - unfold failing issue when cutting

[Lars]

Dear fellow users,
I am facing an issue unfolding a part designed with the sheet metal workbench which is cut into shape with the "Cut" part WB function.
I assume that the root cause of the error is, that the cut function does not cut the sheet metal in a 90-degree angel.
Unfortunately I do not know how to overcome this issue, and hope for your input and inspiration for resolving the error and unfold the item successfully.

Top side ver10 - Forum.FCStd

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Sincerely

Lars


OS: Windows 10 Version 2009
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.19.24291 (Git)
Build type: Release
Branch: releases/FreeCAD-0-19
Hash: 7b5e18a0759de778b74d3a5c17eba9cb815035ac
Python version: 3.8.6+
Qt version: 5.15.2
Coin version: 4.0.1
OCC version: 7.5.0
Locale: English/United Kingdom (en_GB)

[Shalmeneser]

You need to refine the piece if you want to even unfold Bend002

[Shalmeneser]

Code: Select all

Error Analysis: Sheet thickness invalid for this face! at Face11
exception at line 2876("'NoneType' object has no attribute 'Edges'",)

Due to the cut, thickness is no more constant. So it's unfoldable.

SheetMetal_Unfold :

Sheet metal should have constant thickness

[Shalmeneser]

You could 'cut' along the border line with a Sweep.

[Lars]

You could 'cut' along the border line with a Sweep.

I also think the issue is related to a thickness which is not constant after cutting. However I can not figure out how to do a cut along a corder line which then needs to be projected on the bended part?
/Lars

[papyblaise]

I have to look a lot and find 2 problems
(I won't call bug out of sympathy with the developer, just not mature yet)
1st: extend does not work well if we do both sides together
2nd: the cut of the radius (dia 146) is wrong if we cut to the edge, so I only make 1/2 piece and leave some mm
Unfold and miror, but when I do "Fusion" I have another bug in the angles

[papyblaise]

1 hour more research and use V20
by placing Extrude parallel to the cap, and leaving 1mm on the round, it works

[-alex-]

Unfold algorythm fails to unfold eliptic edge related to non-normal cut of "extrude" labeled feature.
Here is another workflow, by using Shell + Part_3Doffset workflow, then I've converted the eliptic edge to arcs (or lines here) with BsplineToArc macro. That's not parametric, but the shape is the same with your former part.
The fix of @papyblaise is better to get a circular edge, because it is parametric. But the shape is slightly different compare with the intended one.
IMHO the best workflow here would be to cut your part with a tessellated profile in the sketch of your "extrude" cutting tool, in this way you will get a result which is similar with an eliptic edge, and furthermore parametric.

topside_ver10_DraftFacebinder_BsplineToArc_3DOffset.png (89.61 KiB) Viewed 973 times

Top side ver10 - Forum-alex-.FCStd

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[-alex-]

Here is your former part, just with tessellated cutting tool. It is fully parametric and success to unfold. Enjoy

Top side ver10 - Forum_tessellated-eliptic-edge.png (41.2 KiB) Viewed 936 times

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OS: Debian GNU/Linux 10 (buster) (LXDE/LXDE-pi)
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.19.24102 (Git)
Build type: Unknown
Branch: master
Hash: 4d3ecdab68399d727efeb8495ede11a2d85f46b0
Python version: 3.7.3
Qt version: 5.11.3
Coin version: 4.0.0a
OCC version: 7.3.0
Locale: French/France (fr_FR)

[Lars]

Dear Alex and @papyblaise,
Thank you for your kind assistance for resolving this issue. Truly grateful for your support, experience and creativity in applying Freecad.
I would not have thought of this solution myself - successfulyy unfold the sheet metal part by changing an arc of elilpse (projected circle arc) into a series of lines by applying a discrete function.
Compared to the version prepared by Alex, I need an increased resolution of discrete version of the arc in order to fit it another part.
For some reason I did not manage successfully to reproduce the sketch of the discrete version of the ø416mm arc in reference mode, following connecting a high number of equally an connected lines along the reference arc.
The sketch menu claims that the sketch is over-constrained?

Top side ver10 - Forume.FCStd

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However, I successfully applied the discrete function in the curves workbench to the body used to cut the sheet metal in shape. The final part cut into shape with the extruded part could successfully be unfolded.

Top side ver10 - Forume.FCStd

(61 KiB) Downloaded 27 times

/Lars

Here is your former part, just with tessellated cutting tool. It is fully parametric and success to unfold. Enjoy


Top side ver10 - Forum_tessellated-eliptic-edge.png
Top side ver10 - Forum_tessellated-eliptic-edge.FCStd

OS: Debian GNU/Linux 10 (buster) (LXDE/LXDE-pi)
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.19.24102 (Git)
Build type: Unknown
Branch: master
Hash: 4d3ecdab68399d727efeb8495ede11a2d85f46b0
Python version: 3.7.3
Qt version: 5.11.3
Coin version: 4.0.0a
OCC version: 7.3.0
Locale: French/France (fr_FR)