Sweep, preview seems correct but final shape is incorrect

[galou_breizh]

Dear all,

I have a problem with the Sweep tool of the PartDesign Workbench. The shape seems correct in the "Edit pipe" context menu but when I click "OK" in this dialog, the obtained shape is incorrect. It appears that only the part of the shape which is within the support cylinder is kept.

Preview

preview.png (37.32 KiB) Viewed 332 times

Final shape

final_shape.png (25.66 KiB) Viewed 332 times

Am I doing something wrong? Does some of you have the correct final shape with another version of FreeCAD?

Thanks,
Gaël

OS: Ubuntu 18.04.5 LTS (i3/i3)
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.19.
Build type: Release
Branch: unknown
Hash: b5dc3887db550faa64b03377b901ef40dc07c970
Python version: 3.6.9
Qt version: 5.9.5
Coin version: 4.0.0a
OCC version: 7.3.0
Locale: English/UnitedStates (en_US)

[kisolre]

Seams
The plane of the profile sketch is coplanar with the cylinder seam line. Seams are how the surfaces are represented by the OCC kernel. You can either move the seam (make the circle from two arcs in Sketch004 OR rotate Sketch004 around its Z axis) or rotate the Sketch005 around its Y axis to move its plane away from the cylinder seam..

[Bance]

It's a co-planar issue revolve sketch by 1 degree and the sweep succeeds.

[galou_breizh]

Good to know! Thanks, experts!

I solved the issue by moving Sketch004, the sketch generating the cylinder, by 90° about the z-axis.