Is there a way to intersect two parts?

[dgore]

Hi,

i want to intersect two parts with the boolean operation "AND". So i need the overlapping geometry of the two parts.

I found the "Component Operations"-Option in Assembly-Mode, but it seems to me there isn't a option similar to the boolean operation "AND".

Any ideas how to do that?

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[dgschaefer]

If I understand, you want to combine two parts into one, correct?  You can do this with the "Merge/Inheritance" function in part mode or the "merge' operation in assy mode.

Doing it in part mode eliminates any parent child relationships between the merge and an assembly but requires a coordinate system (or using default placement) to locate the parts together. Doing it in the assy uses their relative placement in the assy, but makes the assy a parent of both parts.

In both cases, it takes the geometry of one and adds it to the other. If you want to create a new part with the geometry of both, you'll need to create an empty part and perform the merge operation twice to bring in each of the other two parts.

[JonathanHodgson]

Boolean operations are generally done using surfaces (quilts) in Creo / Pro/E.

If you want to "AND" the two parts, you'll probably have to do something like:

• Create a copy of the surface quilt of each part (within the part itself)
• Create a Publish Geometry of the copied quilt (within each part)
• Create a new part and create a Copy Geom referencing each Publish Geom
• Merge the two quilts together (by toggling the 'kept' side of each quilt, Merge can perform AND, SUBTRACT or OR between two closed quilts, I believe)

What's the application?

[mbonka]

Hello some related links:

https://www.youtube.com/watch?v=_Nb0Um5Jui4

Assembly Component Operations - Cut Out PTC Creo: - YouTube

[JonathanHodgson]

Thanks, that's useful to know and is certainly neater for a "cut out".  I also noticed "merge" in the menu - does that correspond to a quilt merge, giving the possibility for both "union" and "intersect" (per the diagrams posted elsewhere in this thread) or does it only do one of them (and in that case, which one)?

[dgore]

OK, thank you that was what i was searching for.

To make it clear for the others, see attached picture.

But isn't there a simpler method, to do it?

[dgschaefer]

You can skip the publish geom step and copy the surfaces directly, but other than that, no, there's not a simpler method to create the "intersect' from your image.

What I suggested above will create the "union" in you image.

[DeanLong]

Or...create the "two" things you want to Boolean as two separate surface(s) (Quilt) first and then merge with the desired Flavor. (I.E. Union, Difference). In Creo, you do not have to start with a solid feature.