How to use a feature in a part in assembly mode to cut a hole into another part

[ptc-4771490]

Hello

I have to apologize if this has been asked before but I didn't really know what to type in search.

But yeah, the thing is I have two geometrically fairly complicated parts that lie on top of each other in assembly. I need several screw holes that connect these parts together but it is hard to pin point the exact location of these holes on both parts since I have used sheet metal/unbend to be able to create the holes on one part and I would have to unbend the other part as well. I was wondering if there is some way I can use the hole pattern feature I have one on part to create the holes to the other part in assembly mode (so that the hole axis are the same).

This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.

[TomD.inPDX]

It is possible to make the holes in the part as described here: but maybe just place points in those locations. Then go into the part and locate the holes un the sheetmetal module so you maintain the unfold capabilities.

If you later dimension the holes fully and remove the dependency of the points, you can then delete the points and thereby also removing the dependency to the assembly and the other part.

Please keep these discussion in one location so others can follow along.

[TomD.inPDX]

BTW: this is not an assembly cut. The hole should be created in the original part -if- you have the part Active in the assembly.

[vzak]

If you want holes in part_B to follow exactly holes in part_A when they stick in assembly you might do this in several ways, 2 of them below :

1. Activate part_B, create Axis feature referencing pattern leader Hole geometry from part-A. Create RefPatern of Axis in part_B. Create Hole in Part_B referencing leader Axis and Refpattern Holes as well. This design will ensure your hole patterns always stick togather when they see each other in assembly.

2. Same as above, but instead of creating an Axis in part_B create Copygeom feature and copy Axis from leader Hole in part A. All the rest - the same. Just design will be more stable.