An extruded hole in a part while in assembly mode doesn't carry over to my part file?

[Tony Bombardo]

Hey Everyone,

I'm still in the process of learning all the ins and outs of Creo Parametric and I've got a bit of a weird behavior going on that I'm assuming is fixable if someone could maybe help me understand it a bit better...

Coming from a Creo Elements Direct background, I'm used to being able to create an assembly, have something like two sheet metal pieces lay flat against each other, then punch a hole in each part at the exact same location for a fastener to go through (Here's a simpler example: I have a 1x1" block with a .5" hole in the center. I then create another 1x1 block with no hole in it. I then assemble both blocks stacked on top of each other and try to use the geometry of the first block's hole to punch the same hole into block two. The result is a stack of two blocks with holes in them that are aligned to each other perfectly. However when I right-click block two in the model tree and click "open" , the part that opens is still the original no-hole block)

I just tried this in Parametric but I noticed that the part I punched the holes in doesn't update or retain those holes in it's original model file when I open it, so I'm left with a part change that doesn't seem to carry over into any files that I could then go and create new prints of.


My theory here is that when I create an extruded hole in the parts in my assembly, I'm more just creating a feature rather than actually changing the part (even though it looks like it) ? any way around this?

The more I learn about Creo Parametric, the more I like it, but I also miss a lot about Direct...

 

[michaelpaul]

features made in an assembly are native to the assembly, not the parts. if you want the hole to be in the part, right click the part to activate it. then you can use the edge of the first part to create a new cut in the active part.

 

[dr_gallup]

Thee is an option in the assembly hole to have the hole in just the assembly level or in both the part and assembly levels. Normally, I consider it bad practice to create the hole in the assembly and show it in the part. It creates a reference to the assembly which may get broken if you reuse the part in another assembly. I tend to use and reuse parts for decades and avoid external references like the plague.

 

[dgs]

There's a modeling philosophy at work here. The assumption is that features created in the assy are features that you would physically create with the two parts assembled. In that case, the parts are manufactured with no holes and the holes don't exist until they are assembled and the holes are drilled, so that's what Creo creates.

As dr_gallup mentioned, there is a toggle for making the assy feature visible at the part level. I would agree, however, that doing so is not the best modeling practice. If the part is made with the hole, build it with the hole.

If you're concerned about maintaining the relationship between the holes, there are top town design techniques like skeleton modeling or the master modeling made for this that better handle the external references.