Model breaks after union

[Fixtor]

This is not the first time it happens to me. I have no idea how to fix this. Can someone help me? It looks like a bug. Happened after making an union.

This is how it should look (before union)

This is how it does look (after union)

Thanks in advance. I hope there's an easy workaround.

Edit: added the file

[quick61]

Pad006 is a BAD model. FreeCAD should NOT allow you to do that, but it does. Part Design is for the creation of a single solid part, not multiple parts from one sketch. The result of doing such a thing as you have done is create a long list of geometric errors in the model that may not show up at first, but as you have found out, will come to the surface later on in the models history. Sketch006 must be split into 2 separate sketches if your going to construct this model as a Part Design / CSG hybrid. Though you probably would be much better off staying with just Part Design Workbench for this model sense it is simple enough and nothing I see would dictate the need for using anything else.

Hang on a few minutes and I'll post an example.

Mark

[Fixtor]

Hey Mark, thanks for your reply! I fixed those issues but the model still breaks, so I have a question. Is this sketch a solid part? Or should I create this square hole with another sketch?

[quick61]

That sketch should pad and work properly.

As I said, that part can be make using just the Part Design Workbench. I did it with 3 sketches and a mirror tossed in to make things easier. The end result is a single part with no geometric errors being reported.

Here is the file -

Sketch_Built_Example.fcstd

(34.24 KiB) Downloaded 14 times

You can take a look at the first sketch as it basically does the same thing as your sketch does, but with a bit more detail.

I first did the base part, then one side of the 'C' bracket, Mirrored it horizontally, then placed the end tab with the 3rd sketch.

Mark

OS: Kubuntu 14.04.1 LTS
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.15.4535 (Git)
Branch: master
Hash: c2d0857ddcba6fc20319a541bfda3fb834e00418
Python version: 2.7.6
Qt version: 4.8.6
Coin version: 4.0.0a
OCC version: 6.8.0.oce-0.17-dev

[DeepSOIC]

Looks like this is the first boolean operation fail caused by coplanar faces I've seen so far .

[DeepSOIC]

Fixtor, BTW, what version of FreeCAD are you using?

I was able to fix the model. In Sketch007, I reassembled all tangent joints to point-to-point tangency instead of coincident+tangent. There were a few (some were proper). I also did this to Sketch, where all tangent joints were correct, but it was the thing that actually cured the boolean.
So it looks like it is solver precision issue here. I might do a further investigation on this.

broken model repaired.FCStd

(63.52 KiB) Downloaded 10 times

EDIT: PS. Fixtor, please! upload the pictures directly to the forum! I feel myself a bit in danger when following the links to unfamiliar websites.

[Fixtor]

OS: Mac OS X
Word size: 64-bit
Version: 0.14.3703 (Git)
Branch: releases/FreeCAD-0-14
Hash: c6edd47334a3e6f209e493773093db2b9b4f0e40
Python version: 2.7.5
Qt version: 4.8.6
Coin version: 3.1.3
SoQt version: 1.5.0
OCC version: 6.7.0

Sorry about not posting pictures on forum!

[DeepSOIC]

Fixtor, thanks!
I have measured the distance between two points that should become coincident, and got a value of ~4.5e-07. This is slightly above OCC's Precision::Confusion, which is 1e-7 AFAIK.
Any sizes that come close to Precision::Confusion are evil. For the stuff to work reliably, the distances should either be a couple orders of magnitude larger (and thus definitely non-coincident), or a couple orders of magnitude smaller (thus definitely coincident).

It looks like it is coming from Sketcher solve errors. They are unavoidable, and it is a bad idea to precisely replicate the shape by making two sketches identically constrained. Instead, the constraints should be to links to external geometry (in this case, the coincidence precision better than 1e-7 is essentially guaranteed).

[DeepSOIC]

Interestingly, on my repaired version of the model, the coincidence is bang on. i.e. I get exactly zero distance. Fascinating

Here's my method of measurement.
Select two points and type the following into python console:

Code: Select all

(Gui.Selection.getSelectionEx()[0].SubObjects[0].Point-Gui.Selection.getSelectionEx()[1].SubObjects[0].Point).Length

To select the two points that occupy the same space, I select one of them, hit space to hide the object it belongs to, and Ctrl+Click the other point.

[tanderson69]

Here's my method of measurement.
Select two points and type the following into python console:...

If you turn on your report view and use part/measurement, you can achieve the same result. Conditions like this were the whole purpose behind writing that command.

measure.png (237.5 KiB) Viewed 1116 times