[FIXED] Ticket #5917: Polar Pattern "transformed shapes do not intersect support" (upstream OCC bug)

[Sembazuru]

I'm trying to design my own makercoin blank and am having issues creating a complex curve shape around the edge. The main coin shape is from a revolved sketch. I then have a Groved sketch (using the coin sketch references for position and size). When I then try to apply the groove as a polar pattern I get the error of transformed shapes do not intersect support, but clearly all the arrayed grooves clip the revolved sketch. Here is what it looks like trying to get my preferred number of 13 grooves (just because it is prime and fits well around the coin).

2019-04-17 00_48_36-FreeCAD 0.18.png (489.89 KiB) Viewed 4270 times

If I change the Occurances up or down there doesn't seem to be any rhyme or reason to which arrayed grooves work and which don't.

For reference, here is my object tree for this model:

2019-04-17 00_49_23-FreeCAD 0.18.png (11.68 KiB) Viewed 4270 times

I've also attached my freecad object.

Here is my version info:

OS: Windows 10
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.18.16110 (Git)
Build type: Release
Branch: (HEAD detached at upstream/releases/FreeCAD-0-18)
Hash: f7dccfaa909e5b9da26bf50c4a22ccca9bb10c40
Python version: 3.6.6
Qt version: 5.6.2
Coin version: 4.0.0a
OCC version: 7.3.0
Locale: English/UnitedStates (en_US)

Am I building the case for a bug report, or am I suffering PEKAC?

[HarryGeier]

First observation:

You are right, it does not work with any number of occurences.

Then i thought, the problem is rotating a revolution around a revolution...
I tried by replacing the groove by subtractive spheres. Then i can create a polar pattern , but the result looks weird:

2019-04-17 08_03_17-.png (148.67 KiB) Viewed 4256 times

As soon as i attach even just one copy of the sphere the revolution begins to look strange....

I think the problem lies in the revolved feature somehow.

[kisolre]

We again hit some OCC coplanar/colinear/co_something issue. Moving the center of the arc some distance away from the edge of the base coin fixes the issue (see the 0.1mm dimension). I also CarbonCopied the base sketch as construction geometry just because I came to like that recently:

ScallopedEdgeCoin_offset.JPG (102.41 KiB) Viewed 4252 times

ScallopedEdgeCoin_result.JPG (110.54 KiB) Viewed 4252 times

[Sembazuru]

We again hit some OCC coplanar/colinear/co_something issue. Moving the center of the arc some distance away from the edge of the base coin fixes the issue (see the 0.1mm dimension).

This was it, exactly. Just offsetting the center of the arc vertically from that edge did the trick. Glad it wasn't PEKAC. Now I just need to figure out how to search the bug reports to know whether to add on to an existing report or create a new bug report. That's a task for another night. (I'll be following the instructions posted on this forum here, so no need to instruct me.)

BTW, how do you get the transparency effect on the object? I've tried several things and not gotten that look. But I want it.

[kisolre]

RMB->Appearance over the body in TreeView.
OCC bugs should be reported to OCC bugtracker. Which as I understand it is a tedious process. The guys there are aware of those issues and probably working to fix them but untill that happens... And is included in FreeCAD,...

[NormandC]

This kind of bug is well known and most probably caused by OCC, over which the FreeCAD developers have no influence, it's a third-party library. On the other hand having this registered on the FreeCAD tracker with the file attached would allow us to test it when new versions of OCC come out. In the forum it will be forgotten.

To report bugs to OCC basically requires to be a developer, a script working with their test program DRAW.exe must be provided.

[jmaustpc]

Norm is right, but also keeping FreeCAD examples of occ bugs makes it easier for someone who has jumped through the hoops that occ expects someone to go through to contribute to occ, to produce a bug report or even a patch etc. at occ.

Also an occ dev was here on our forum recently, I can't remember his name just now. Do you remember Norm? If not I'll try to find it tomorrow, he might be interest in FreeCAD occ bugs possibly.

Jim

[chrisb]

Do you mean Quaoar?

[NormandC]

Just to make sure the issue is not only with PartDesign's MultiTransform, I copied the groove sketch into a separate Body and created a revolution to get a sphere; I used Draft Array with 13 instances with rotation axis at (0,0,0) then applied a Part Cut between the first Body and the Array; the model shows the same issue.

In the OpenSCAD workbench, there is a "Increase Tolerance Feature" entry in the OpenSCAD menu; I though by creating such a feature and editing its tolerance values it may be possible to make the cut succeed; but I've never used this feature before, and was not successful.

[Sembazuru]

This kind of bug is well known and most probably caused by OCC, over which the FreeCAD developers have no influence, it's a third-party library. On the other hand having this registered on the FreeCAD tracker with the file attached would allow us to test it when new versions of OCC come out. In the forum it will be forgotten.

To report bugs to OCC basically requires to be a developer, a script working with their test program DRAW.exe must be provided.

To be honest, I as a simple end user (and an overall simple person ) have no concept of what OCC is, or that it is a third-party library. So, I'd be inclined to post the bug report where I see it, namely in FreeCAD's bug tracker.

I just submitted the bug here: https://www.freecadweb.org/tracker/view.php?id=3938

Interesting experiment with OpenSCAD workbench, but FWIW I don't have OpenSCAD installed here. (I know the OpenSCAD WB comes as default, but the WB is the only thing with the name OpenSCAD installed on my computer.)