Creo 2.0 - Copy Geometry

Two suggestions:

1. If you simply want to temporarily reference the bolt, a copy geom feature is overkill.  In the assy I'd activate the part you want to put the hole / cut in, start a new hole or extrude feature and select the bolt's diameter or center axis as a reference and create the feature.  Then, open the part independently and redefine it to remove the reference and tie it to what you want.
2. For a more robust assy, look to using top down design with a skeleton.  You'd place a datum point or axis in the skeleton and pass it down to the two parts being joined and create your hole off of that.  Then, if the location needed to change you'd change the skeleton and the parts would update.  This would require  using a copy geom feature, and possibly a publish geom feature, to pass the geometry from the skeleton to the parts.  More work, but more robust adn flexible in the long run.

You'll find the copy geom feature in the "Get Data" area of the model tab.  Activate the part in the assy and select Copy Geom.  By default, it looks for a "Publish Geom" feature, which is a predefined set of geometry in the source part that you want to share.  Unclick the publish geometry button (a box with 3 arrows) and then you can pick specific geometry items to be copied into your part.

You can do the same outside of the assy, you just need to pick the source part first and decide how to align them.  This eliminates the assy as a parent.

If you want to pre-define geometry to share, you can create a publish geometry in your source part first by looking under "Model Intent" on the "Model" tab.  The interface is the same as the copy geometry.

There is a decent, but old, tutorial on skeletons using an office chair in the PTC knowledge base, look that up.

Yes Steven, I'm trying to locate a new hole so that later i can assemble the bolt into it, knowng it is in the exact place i want it to be.

The green bit is a plate...i want to accurately locate a hole to tap that is in the exact place the yellow bolt is.

In wildfire I would have activated the the green plate and simply created a copy geom of the yellow bolt surface and then go into the plate part, draw the hole and then tap it or whatever, but the point is i was able to use edge, which i can't do now. Even if i activate the plate within the assembly it still won't let me use edge or select any surface or edge to create a sketch from....for me, the functionality has been utterly ruined.

Thanks!

I can get as far as the image you posted Steven, but I can't select anything......

I can now select stuff but the copy geom is a no go even with the correct License.....

I copied Multiple surface from one part. After that I forget the location of the part. Now I want to locate that part. Is there any way to find the location of the copy geom part.

Have not used Copy Geometry before but was able to follow Doug's instructions and get geometry copied over to the part:

• You'll find the copy geom feature in the "Get Data" area of the model tab.  Activate the part in the assy and select Copy Geom.  By default, it looks for a "Publish Geom" feature, which is a predefined set of geometry in the source part that you want to share.  Unclick the publish geometry button (a box with 3 arrows) and then you can pick specific geometry items to be copied into your part.

Your screen shot looks like you selected the wrong button.  Select the last button to turn it off.

The method I have been shown that eliminates any external references, and does not require AAX, is to select the surfaces wanted and use Ctrl+C & Ctrl+V to create a surface Copy in the assembly.  Next save a Copy as an IGES and select the copied surface by selecting the Quilts button then the surface and use the destination parts CSYS by selecting the arrow button in the Coordinate System box then the destination parts default CSYS.  Open the part and use Import under Get Data to import the surface.