Possible problem in drawing. Missing lines

[dcapeletti]

Hello, I'm attaching the file so you can verify it.
I enclose an image where I mark the missing line.

If it's a design error, I'll be grateful for your recommendations. I hope you can help me.

Thanks

OS: Debian GNU/Linux 9 (stretch) (GNOME/default)
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.19.17445 (Git) AppImage
Build type: Release
Branch: master
Hash: 741dddf25485f692596faa9b7911e2e0f5d362a3
Python version: 3.7.3
Qt version: 5.9.7
Coin version: 4.0.0a
OCC version: 7.3.0
Locale: Spanish/Argentina (es_AR)

[wandererfan]

I enclose an image where I mark the missing line.

If it's a design error, I'll be grateful for your recommendations. I hope you can help me.

I think it is an OCC error in either the HLR algorithms, the Projector algorithms or both.

In your file, you are using Coarse View for FrontBottomLeft and Detail. (Coarse View uses the polygon approximation version of the HLR with the orthogonal Projector.)

If I set CoarseView off for FrontBottomLeft, I get your missing line back (red arrow), but also get some hidden lines being visible (blue arrows). I also get an extra red line(?!). (Precise version of HLR with orthogonal Projector).

PreciseArtifacts.png (63.84 KiB) Viewed 295 times

I get the best results by setting CoarseView off, Perspective on, and focus length of 1000mm. This collection of options uses the precise HLR with the perspective Projector.

Engranaje_Perspective.png (252.14 KiB) Viewed 295 times

Can't see any obvious design errors, but it is good practice to use the Body as the Source for TechDraw Views, rather than one of the feature history entries (Pocket001).

[dcapeletti]

Can't see any obvious design errors, but it is good practice to use the Body as the Source for TechDraw Views, rather than one of the feature history entries (Pocket001).

Thank you for your help and advice.
I've done what you tell me, but I still get errors in the projection. I think techdraw should still get some improvements. Are they planned for version 0.19?

Greetings

[wandererfan]

TD/OCC always struggle with invalid shapes.

The first feature (Pad) in your chain fails Part.checkGeometry. The InvoluteGear passes, but PartDesign Pad and Part Extrude both create shapes that fail.

engranaje_checkGeometry.png (175.85 KiB) Viewed 199 times

If I take a copy of InvoluteGear, convert it to a Sketch with Draft, then use Part.Extrude on the Sketch, I get a valid solid that passes CheckGeometry and draws nicely in TD.

Engranaje_PadFromSketch.png (29.32 KiB) Viewed 199 times

I don't know why the original is invalid, but the manipulated version is good. Maybe there is a Sketcher/Part Design expert that can explain.