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Holes in assembly or part


New member
I want mating holes between two parts. What is the easiest way to do it and get the information into the part model. I did it in assembly, but it didn't go top-down into the part.

I'm doing a lot of modeling in Assembly mode (external references), which I realize is a no-no to some shops - but to me it seems like the whole point of top-down design (on a moderately simple assembly).




The easiest way to do it is to create a hole in the correct positon in one part, then go to the assembly.

Activate the mating part, and make the hole on the correct face, and use co-axial for the reference, as opposed to linear - it's in the Placement menu in the dashboard.


New member
It's pure engineering logic. It depends how do you plan to machine those two parts. When you need to draft shop drawings of those two parts without holes (e.g. for plasma cut-out) it is convenient to create assembly feature, other wise you could create hole features in parts and relate them with assembly relations.


New member
Another hint

Becarefull if you work in assembly .......

if you have a lot of holes and you must do hole tables ............if you have 40 or more different holes is easier to create the holes starting from the corect face

I think here abbout machinning you must do after



New member
My opinion, if someones interested:

Creating holes for example is great in assy mode if you are doing one-offs design, like machine equipment fixtures or similar.

When you use your components inseveral different products I wouldnt use this technique.

Imagine that you use a bolt pattern in one component as a reference when creating a bracket. That bracket is of course a very good one so your colleagues put it in their products as well.
After a while you decide to use another bracket and adapt your bolt pattern to match. Dont think I need to write what happens with the original bracket then.....

So my answer to the question is that it depends of what part you are making. Is it a generic dont use ext refs, is it a unique design assy mode is great.



New member
for a "full power" flexible approach:

share a skeleton.

I like to sketchdatum curves in a skeleton (features of skeleton component or assembly features) in the assembly. then you can data share them to the parts. INSERT, SHARED DATA, COPY GEOMETRY FORM OTHER MODEL. near endless list of options for this such as: dependant, independant, how they are located etc...

then use those curves to locate (and or size) the holes in the components.

as a bonus, the copies can be independant, and not need to pull the skeleton to regenerate, BUT can be made dependant at a later date if you want to automatically update them.

Warning: i hear some PDM systems STILL reference and retrieve the skeleton and the assy even when independant?


If you want, you can change the assy hole feature to intersect the parts at the part level rather than the assy level. However, you will have to pull up the assy when you want to work on the part. Skeletons for top down design work better than lots of external references in assy mode. You are living dangerously.


New member
dsergison, Intralink does that, that is references independent geometry from other parts. It shows that independent referenced part is a ghost object, but when you checkthe assemblyin, it breaks the dependence between the origin of references and the copied references part.