How to Project Hole Locations from One Part to Another in Creo Assembly

[ENGINEERINGXYZ]

I'm currently working on an assembly where I need to ensure that the hole locations on two different parts are identical. Specifically, I want to project or reference the holes from Part B onto Part A within the assembly. I've explored a few options but haven't found a straightforward way to achieve this.

Any help or advice would be much appreciated!

[Tdaugherty]

If you are cool with external references (like me), you can reference the mating part directly to create your hole. Activate the part you want holes in, select the axis reference in the mating part and then select a surface to place the feature. This will create a reference between the two components and ensure that the holes always line up in the parts move relative to each other. 

If you don't like external references, you have a few options:

• sketch the bolt pattern in both parts and ensure they line up - requires babysitting
• publish/copy geometry
• reference backups - allows you to use my preferred method from above but control update behavior (you can break the link this way)
• skeleton - can be used to drive geometry in both parts 

[tbraxton]

If you are new to Creo I would encourage you to avoid creating assembly references unless there is no other way to capture your design intent. If you ever work on designs of even medium complexity, assembly refs can haunt you.

An external copy geometry feature from the model with holes (B) would be a good way to handle this with part B being a parent of part A and not having to have the assembly in memory to modify either part.

[tbraxton]

Watch the video in this thread for one example of how you can deal with this problem in Creo using external copy geometry (ecg) functionality. This deals with intermediate to advanced functionality that leverage the power of Creo to deal with this type of shared design intent problem. Watch the whole video as it demonstrates what is possible by leveraging some of the Top-Down tools.

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[Hidetaka]

The best way I know to achieve what you want is to use skeleton model. 
If you are using top down design approach, there is no problem with referencing skeleton model features.
To make sure that two holes on two parts are always aligned, just use Creo hole feature, and use an axis in the skeleton model as common reference for both holes.