How to use the intersect tool for two components in an assembly with solidworks?

Question

I have an assembly file in Solidworks 2019 with two components, the green, and yellow rectangular prisms.

I'm having trouble understanding the instructions I found online about making an intersection with these two components. Can someone help me with this?

They form a subassembly in a larger file, and I'm really just interested in the volume that they share.

Edit I just found out how to make a 3D sketch outlining the intersection. Tools > Sketch tools > Intersection curve. But I'm not sure how to take this further and extract the intersected volume.

Edit 2 I am looking to take these two parts from the subassembly and make a new single part where they intersect.

Yes, they ultimately do need to be an assembly, but if it can be converted temporarily that's fine. It can be saved under a new name first as a file with a multibody if necessary.

The only remaining part should be the intersection of yellow and green. (Although if I think about it carefully, it might be important not to remove the portion of green below the intersection in the final part.) The leftovers can be removed as long as it's in a separate file. I still need the subassembly for other things in the larger assembly I mentioned.

Answer 1

So, this is actually non-trivial. Here are the key points:

1. In order to use the "Combine" feature, to create the volume that you want, you need to have a multibody part

2. In order to move the parts dynamically inside a multibody, you need to use mates with the "move/copy bodies" feature. It cannot accept a global variable for translate/rotate moves, which is a bit annoying.

3. You cannot mate to an external reference, therefore, the position of the parts in the assembly must be defined by the position of the parts in the multibody, not the other way around.

I have created a demo assembly here, which I believe achieves all of your goals: http://www.filedropper.com/yellowgreenintersect

The way that this works is as follows:

1. The green part is fixed at the origin in both the assembly and the multibody - you can follow the same method as explained below for the yellow part if this is not suitable

2. I created a virtual component for the intersection, and used "Insert Part" to insert both yellow and green parts at the origin.

3. I created a 3D sketch to fully define the position of the yellow part. Adjusting the geometry of this 3D sketch can control all six degrees of freedom. Currently it's dimensioned for X/Y/Z position, and the rotation is fixed by constraints, but if you were to remove these and place angle dimensions, rotation could be controlled also.

4. I used move/copy bodies to constrain the yellow body (inside the multibody part) to the 3D sketch

5. I used the Combine feature to create the common volume (Red)

6. In the assembly the Yellow body is mated to the 3D sketch from the part, using the same constraints. If you want to move the yellow body position, you must edit the 3D sketch.

7. Everything updates dynamically, you can change the shape/size/position/rotation of the bodies, you can add bosses or holes etc.

I hope this helps - good luck!