First of all I apologize if I have discussed this topic before. I tried doing a search on this but couldn't find how I could view all my discussions.
I do not like how difficult it is to take model changes through new modifications; the struggle is with the naming.
I componentize my models. The 1st model is the basic shape. The 2nd model adds flash at the parting line. The 3rd model places gutter depth beyond the flash width. The 4th model assembles all of this in a die. I have to put several componentized model sets into the final die.
The changes themselves I would consider as going through this process very easily (most of the time).
The struggle is the fact that each of these models needs name changing to identify the new revision number.
To discover how to even make this go through was a struggle in itself, but now I at least have a method that will update component by component. This process takes hours.
I'll lay out the left and right jobs that I just did to illustrate the mounting frustration I have with this process. You don't have to wade through the next 44 steps but it shows the pattern I have to follow so the change properly filters through all of the components.
1) Change base model of 1st stage
2) Bring base model into flash model
3) Go back and change base models name and make sure new name loads into flash model
4) Go into gutter model and bring in flash model change.
5) Go back to flash model, change it's name and make sure new name loads into the gutter model
6) Bring gutter model into pro-mold die as bottom and top impression.
7) Change name of gutter model and make sure it comes into die.
😎 Open up and change name of top and bottom impression reference models.
9-16) Repeat this process for 2nd stage
17-24) Repeat this process for last stage
25) Change name of die and anything within die that includes the new change number
26) Go to opposite hand 1st stage gutter model and review the number that the model wants to import.
27) Change name of the previously changed gutter model to line up with what the opposite hand gutter model wants to see (name prior to change)
28) Bring the 1st stage gutter into the opposite hand gutter model
29) Bring the 1st stage gutter of the opposite hand into the die
30) Go back the 1st stage opposite hand gutter model and modify it's name to the new revision and make sure this number loads into the die in pro-mold
31-35) Repeat same process for the opposite hand of the 2nd stage
36-40) Repeat same process for the opposite hand of the 3rd stage
41) Change name of die and anything within die that includes the new change number of the opposite hand die.
42-44) Change back the name of all the original gutter model files to reflect the true release number.
This is time consuming and breeds opportunities for missing something and making mistakes.
The same process with our other CAD system is much simpler.
1) Change base model of 1st stage and save it
2) Bring this into flash model and save it
3) Bring this into gutter model and save it
4) Bring this into die and save it
5-8) Repeat this process for 2nd stage
9-12) Repeat this process for 3rd stage
13) Go to opposite hand base model 1st stage and bring in base part originally modified and save it
14) Bring this into die and save it
15-16) Repeat that process for 2nd stage
17-18) Repeat that process for 3rd stage
Not being able to replace out names of inserted components causes huge headaches.
I have a couple questions;
1) I have to be able to verify that my model changes have been brought all the way through; is there a simpler way to guarantee this?
2) How many out there struggle with this same issue?
Solved! Go to Solution.
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.
Are you using the Mold/Casting application inside Creo for this? If so, are you using the reference model capabilities? You should be able to swap out the part geometry in the reference model and have the mold components update...
I have no trouble with geometry updating with changes. My issue is when there is a name change to the geometry that gets inserted into the die.
You would have to make sure the upstream models carry the geometry changes and insert into the die. Then you would change the upstream model names before they would cleanly integrate into the die.
I've tried different ways around this but if you want to retain the shape of the reference models (which would in themselves have changes) you would have to go in the order I've described.
I would love to be proved wrong, but I've tried the following methodology and it falls apart when the reference model was changed in the die.
First, make sure that the ref part is unblanked in the assembly. Then right-click on the ref part and click Replace, as you have already done. In the Replace window, click Unrelated Component then select the “file open” icon in the Replace window to select your replacement model. Then pick Edit Ref Table, which will allow you to map references between the ref model and its replacement. With any luck, you will only have one coordinate system as the reference and you can pick “Evaluate” and be done with it. Occasionally after replacing a model you may have to redefine any failed features due to missing or radically changed references.
Could you please post a video of the process? This just seems way too complicated, guess it'd make a long vid.
I wonder why the Replace option fails.
Yes the whole replace routine would be a very long and confusing video.
I hope a series of snapshots will describe this confusing process.
Below is the starting model.
Which gets fitted in the below part model.
The quandary develops when I have to retain the naming of the base model; otherwise I can't replace out the needed model. (Nothing will show up in the replacement box)
Below is the blocker models inserted into the gutter model.
Below shows gutter models inserted in the die.
Notice that there still is an issue of matching up part model names.
These pictures illustrate the progression of the tedious name changing as explained in my original post.
Hopefully this shows the unnecessary struggle that needs to be followed in order to carry new changes through our dies.
Even more hopefully there is a way around this, or it might be changed in a future Creo release.
As you already know, It's not possible to replace the model in Merge/Ineritance feature, other than with a family table instance, which is pretty odd.
I suggest building the structure such that you don't have to replace the model inside the Merge/Inheritance feature. It'd be easier if you could redefine a Copy feature made of All Solid Surfaces inside a dummy model that is then being inherited or merged into the die. This copy feature can handle getting geometry from different model each time, it can serve as a middle man. Well, if you are ok with getting only the geometry from the reference models, and not all the features, including datum axes, etc.
If you've got everything in session the renaming should work without any problem, even in your case without when you have models linked with merge/inheritance features. So, I still don't see renaming as a problem there, anyway.
When working in assembly, under Model tab --> Component dropdown --> there is Component Operations command, which lets you use Merge/Inheritance in the context of an assembly, if you choose the Merge option in Menu Manager that pops up. All this takes is to read the Message Log carefully.
That can help you do all of your work on assembly level, so you don't have to open each part separately.
The solution isn't very elegant, but should work as long as everything is in one assembly. I can try to explain it using some examples if you want me to. Btw, have you got Flexible Modeling Extension?
We have different reasons that we like to componentize.
1) To simplify and specialize model feature tree by application
2) The parts need to be split out at different points for different applications. (Mostly to separate forge dies from trim dies) (These models are Family Tabled according to this need)
3) The very nature of multiple varied impressions needed for the die
We have a system now that minimizes the amount of work needed to get the entire job through. It just goes downhill every time we need to make part changes.