This does sound intriguing but I am wondering how easy something like this would replace out. Would the downstream history tree hold together? I'm also wondering if there was a way to verify the version of this inserted feature.
I tried doing this from Assembly as you've suggested but didn't see any kind of a merge prompt. Would you insert the copied geometry at assembly level?
This almost sounds like the Copy Geom command. I've seen this done but haven't tried this myself and I'm not sure how well this geometry can be replaced out.
I don't have to retain the datums or points all the way through, but there are times when I would need to bring through curves for part stamping.
If you've got lic for Copy Geom feature you can make the whole thing independent on the assembly file. You can use Copy Geom instead of Copy feature (that is Ctrl+C and Ctrl+V).
To describe it little further. There is one caveat when using Copy Geom, if I remember correctly, if you want to select All Solid Surfaces you have to click on a source part in the model tree. Of course to get solid you will have to use solidify feature after that.
Imagine a simple example with two parts in an assembly, one has got solid geometry and the other one is empty. Activate the empty one, start Copy Geom feature and click on the first one in the model tree, in the selection box All Solid Surfaces should show up.
Again this makes feature dependent copy, not file dependent like in case with merge/inheritance.
Copy Geom, as well as regular Copy also allows curves to be copied.
EDIT: Well, I think you will still need the assembly file to edit the Copy Geom feature. It just won't do odd things when you open any of these copied parts separately, without having the assembly file in session, like it sometimes happens with Copy feature. Anyway, too much theory.
In as much as what I've seen so far (done by an outside source) the Copy Geom feature traveled from part model to part model. I'm not sure how this would be done if this was through Assembly.
There still appears to be a dependency on the file that the geometry comes from. In one way this is good because it guarantees that you are bringing over geometry from a specific model file. On the other hand it appears you still are bound by the same restrictive change rules that are present with a Merge Inheritance. If I change the model name which I draw from for the downstream model I can't bring this geometry into the downstream model. I have to 1st bring in the original model manually and then change it's model name. So it looks like I'm in the same boat with Copy Geom.
I need to verify that my new base model inserts in the downstream model, but I need to be able to do this just by redirecting the file from the downstream model.
Here is the vid of what I've meant: cheap merge and replace using middle model - YouTube
It's the cheap way with Copy feature, as I don't have AAX, I have to go without Copy Geom and Inheritance.
Today someone in our department edited a die model done on the outside which used Copy Geom features. This did pass the 1st test of cutting out numerous additional operations as you can at least modify the model name which gets inserted into the die. I have yet to see whether the parametrics from the prior Copy Geom feature hold together. Our model did not but the replaced model was quite dis-similar. If by chance this does see identical features from before this could be simpler than working directly in Pro-Mold.
James: The video was a bit hard to follow, but it appears it's purpose was to show that you can copy features while in assembly without using copy geom or inheritance modeling.
I've figured out that i can pull AAX licence from Creo NC licence that we have.
Do you want me to make a recording where Copy Geom is used?
If this could show a way to cut out a lot of file naming gymnastics I would be very interested.
Since you can swap out different file names upon import with copy geom this would appear to help in itself.
See the vid here: copy geom version of replace merge part - YouTube
Hopefully I wasn't going too fast this time.
James: I watched your video and I think I understand what you were doing. It is interesting to see how some one else would do things in Creo; you used different selections that I haven't even tried yet. Not that this has any bearing on the ultimate result I see that you used Copy Geom with Assembly instead of External. Perhaps you just wanted to build the structure completely in Assembly instead of having outlying part model files.
I've been doing a lot of experimentation with Copy Geom with some of the new jobs I've been working on.
As far as methodology with Copy Geom is concerned, you still end up with disconnects downstream if you were to change the name of the model file that gets inserted into another model (due to a revision) and if in Session Management you "erase not displayed". (That would replicate more of the real world change conditions as you likely would have the upstream model already completed already out of the session prior to a real world change.) (Of course you could do all of your downstream changes without dropping the session you were working on, but this is a harder to pull off so I'm going to assume Copy Geom can't parametrically flow downstream with an upstream name change.) The following is the message that you get when you work through the downstream change and the upstream file name was changed.
I've seen that this fails parametrically after an upstream name change.
STILL: I am finding that I prefer the work flow using Copy Geom in die models using part model files for the top and bottom dies, and an assembly model file with top and bottom assembled in position. This to me is preferable in our situation to directly using Pro-Mold. I see several advantages here even without the clear-cut parametrics downstream.
1) Less model files are generated and are in need of change. (There is no work-piece file, there are no files for the internal reference models. Typically 7 less models!)
2) There are less gymnastics required to prepare the models for use in the dies. (You don't have to butcher the reference models inside the Pro-Mold file for end shape)
3) There are less transition nightmares where the die will not split into 2 pieces
4) The work is easier to see
5) Changes are easier to make inside the die without consequences to the opposite die
6) There is an actual option to use undo if you've made a mistake
7) Curves that are copy geom into the die actually don't disappear in the die.
😎 Assembly is a much better interface to work with than the strangely pieced together Pro-Mold
In short I am thinking this will help me work much faster with less possible mistakes by missing something when tying everything together in the name changing gymnastics.
For some users the Pro-Mold interface would work perfectly fine, but in our application it was a big miss and it had us looking at Solidworks or other CAD software just to do the die work. Yes; we won't fully utilize the Pro-Mold package, but Copy Geom appears to be a suitable alternative.