Intersecting contours pocket.

[kisolre]

I was under impression that intersecting contours in a single sketch was not good. Why does the following groove work?
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IntContGroove.JPG (41.78 KiB) Viewed 1381 times

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Trying to pocket with the same sketch fails (multiple solids) or gives wrong faces depending on there I move the circles up/down (still intersecting).

OS: Windows 8.1
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.19.17171 (Git)
Build type: Release
Branch: master
Hash: d19470a9711ea604f3ca6c93e46afadf64d5bb87
Python version: 3.6.6
Qt version: 5.6.2
Coin version: 4.0.0a
OCC version: 7.3.0
Locale: Bulgarian/Bulgaria (bg_BG)

[chrisb]

Can you upload the file?

[kisolre]

Sure. But I thought it was clear from the screenshot... Those circles are in one sketch and grove works perfectly fine. First they were just touching - no problem there. Then I moved them closer togerher and realized that they were intersecting and would probably make just the outer contour from arcs. But got lazy and decided to give it a go. And strangely it worked ?!?

[papyblaise]

Hello
So resolu or not

[chrisb]

Sure. But I thought it was clear from the screenshot... Those circles are in one sketch and grove works perfectly fine. First they were just touching - no problem there. Then I moved them closer togerher and realized that they were intersecting and would probably make just the outer contour from arcs. But got lazy and decided to give it a go. And strangely it worked ?!?

It was clear from the image, but rebuilding with eventually occurring boundary conditions takes some time; so I prefer to use your file. I will fiddle later with it.

[quick61]

Sure. But I thought it was clear from the screenshot... Those circles are in one sketch and grove works perfectly fine. First they were just touching - no problem there. Then I moved them closer togerher and realized that they were intersecting and would probably make just the outer contour from arcs. But got lazy and decided to give it a go. And strangely it worked ?!?

Actually it didn't work. Yes, it "looks" like it did, but run a geometry check, BOP check enabled and the errors show up. Are you "getting away with" it at this point? Probably. Is it a good model? No.

Use the Arcs, and everything checks fine.

Mark

[kisolre]

Actually it didn't work.

The solid that does not pass BOP check is the fillet. Groove passes Ok. I tried groove with arcs and fillet fails again but groove is Ok. Any idea what "BOPAlgo GeomAbs_C0" means?

[TheMarkster]

It's curious that it works with revolve/groove. Maybe that algorithm is more robust than Pad/Pocket.

[TheMarkster]

The solid that does not pass BOP check is the fillet. Groove passes Ok. I tried groove with arcs and fillet fails again but groove is Ok. Any idea what "BOPAlgo GeomAbs_C0" means?

https://people.cs.clemson.edu/~dhouse/c ... plines.pdf

Page 92 seems to explain it. It has something to do with how the curves join.

[Chris_G]

The solid that does not pass BOP check is the fillet. Groove passes Ok. I tried groove with arcs and fillet fails again but groove is Ok. Any idea what "BOPAlgo GeomAbs_C0" means?

From what I understand of BOP Check, it does 2 different things :
- it checks actual errors in a shape
- it also tries to highlight the properties of a shape that could lead to errors if this shape is used in a boolean operation

BSpline curves can have sharp points (and surfaces can have sharp edges) : this is C0 continuity.
( I don't know if other geometries can have C0 continuity ).
I think this C0 Continuity is reported in BOP Check because it is a potential failure condition for some higher level operations.
For example, surface offsetting doesn't work on C0 continuous surfaces.
I think sweeping along a C0 curve can also produce twist.

Attached file is a sketch, that has been approximated to a single BSpline curve (with a sharp 'C0' point), that has been extruded to a face (with a sharp 'C0' edge).
This curve and this surface are perfectly valid, but they may probably make some boolean operations to fail.