Combining hollow and solids

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Saftiger J
Posts: 3
Joined: Fri Apr 28, 2017 11:13 am

Combining hollow and solids

Post by Saftiger J »

Trying to combine by boolean operation, a hollow and one thats not hollow.

The hollow one is from importing a Step-File. The others - some I made myself and some I downloaded.

I select the parts, i press the combine-button and both parts dissappear.

Is it because the part is hollow? how do i "fill out" the part?
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NormandC
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Joined: Sat Feb 06, 2010 9:52 pm
Location: Québec, Canada

Re: Combining hollow and solids

Post by NormandC »

Hello Saftiger J,

Welcome to the forum.
Saftiger J wrote:i press the combine-button
There is no "combine-button" in FreeCAD. I assume you meant Image Part Union?
Saftiger J wrote:Is it because the part is hollow?
It depends on what you mean by hollow. Do you mean it's a model made of faces, with no thickness nor volume? If it is, you should have received a warning before proceeding, telling you that Boolean operations on non-solids can produce unexpected results. But as a test I tried to create a union between a cube and a simple face, and I didn't get the warning... The operation was completed but failed.

If by "hollow" you mean for example a tube with thickness, then it could be an appropriate solid, and the reason the union failed may be something else. You can use Image Part CheckGeometry on your imported part to see if it's a solid or not. You need to click on the "Shape Content" titlebar to reveal its content.

In the Model tree, there should be a "Fusion" object, and over its icon, a white exclamation point in a red circle. Hovering the icon should display a tooltip showing "Fusion failed".
Saftiger J wrote:how do i "fill out" the part?
It's difficult to say without knowing what your hollow part looks like. Which is why in the forum rules (link is in that large clashing and hard to miss reddish box at the top of this page), we ask people to provide their FreeCAD document (*.FCStd).

You can have a look at the Image Part Shapebuilder utility. If you can create a face from existing edges of your hollow part, then you can create a closed shell by combining it with your hollow part, and finally create a solid from the shell.
Saftiger J
Posts: 3
Joined: Fri Apr 28, 2017 11:13 am

Re: Combining hollow and solids

Post by Saftiger J »

first of all, thank you very much for taking the time to help me!

I will try to upload a simplified version of what I am working on.

yes, i meant Part Union.

CheckGeometry gives me this:
"
xxx.Part__Feature001:
VERTEX : 8
EDGE : 13
WIRE : 6
FACE : 6
SHELL : 1
SOLID : 0
COMPSOLID : 0
COMPOUND : 0
SHAPE : 34
"
So I guess its not a solid.

Tried to go the way you mentioned, over Part Shapebuilder. I selected all the edges created a face from it and combined both, yet still when I want to add solids to it I get the mentioned error and the selected parts dissapear.

When i run CheckGeometry on it it says:
"
VERTEX : 8
EDGE : 13
WIRE : 6
FACE : 6
SHELL : 1
SOLID : 0
COMPSOLID : 0
COMPOUND : 1
SHAPE : 35
"
so I guess it's still no solid.

The problem is that there are hundreds of small parts in my imported model and selecting every edge would be lot of work. Although I can use Part Union on those to create one object out of it. When I add other objects - like solids I created of a sketch or 3D Models I get from suppliers, it fails. Probably because they dont fit as smooth together and there is some kind of overlapping going on.

What I am looking for is a not too time consuming way of modifying and trying out different layouts of this kind of boards. If you are able to help me here, it would be very great. If not also thanks again...
Attachments
simplified Board.FCStd
(43.8 KiB) Downloaded 22 times
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sgrogan
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Joined: Wed Oct 22, 2014 5:02 pm

Re: Combining hollow and solids

Post by sgrogan »

Hi Saftiger J,
Saftiger J wrote:When i run CheckGeometry on it it says:
The sample file helps alot. Running Part_CheckGeometry with extra BOP checks activated on Board001 reveals that not only are all your objects shells, but they are all invalid shells.
board.PNG
board.PNG (31.17 KiB) Viewed 1549 times
If you select Edge7 or Edge13 they will be highlighted in the 3D view in green. Also note that in the Shape Content pane 13 edges are reported. A cuboid should only have 12! So all the later problems come from this invalid geometry/duplicate edge.
This exists for all your objects, so the question is how this so repeatedly happens? I doubt that it is the FreeCAD step importer.

I did find a painful way (because you have so many objects) to fix the geometry.
1) Select the object and use Draft_Downgrade This explodes the invalid shell into valid faces.
2) Multi-select all the face and Part Union them. This results in a valid shell.
3) Select the Fusion and Part > Convert to solid This results in a valid solid that is suitable for further operations.
4) Re-label the solid Board001 to preserve identification.
5) Delete the unnecessary stuff.

What is needed is one of our scripting guru's to write a script that loops through all your objects to accomplish this efficiently.
For someone who might try, there is a command "Fuse compound" in Lattice2 that fixes the shell.
"fight the good fight"
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