Is there a strategy to redo your part to "clean up" the model tree?

[AB_10071442]

I was developing my concept for a part within creo, so I made changes here and there until I had a part that I was happy with. But now, the model tree is very large, although it would now be possible to make up the model by a simpler model tree and less construction elements. Is there a way to keep the outward geometry of my part but change the model tree, to simplify it?

One suggestion that I had would be to create an assembly with the complicated part and create the simple part on top of it, but then my new part is not independent but has references to the old part. Has somebody maybe done this before and knows a hint on how I could simplify my part? 

[tbraxton · Accepted solution]

I think you are asking if you can retain the envelope of the solid geometry and reverse engineer it in a new model. If that is what you want to do, the most simple method would be to save the current part as a Creo neutral file and use it as a template in a new model. This will provide a visual template for you to reference. The one caveat is that you must be diligent about not using any of the import geometry as a reference of your new features.

Once you save the neutral file you will be able to import it into a newly created start part using Model->Get Data->Import . You will then see it as a neutral import feature in the tree. 

The imported geometry will show as an import feature as seen here. I suggest you put it on a layer and create a mapkey to show/hide the layer. This will make it easier/faster for you to avoid using it as a reference.

You can align to the import geometry when creating sketches to quickly replicate the geometry needed but you will need to delete those references  in sketcher and constrain it using the new design intent. This will allow you to delete the import geometry when you are finished and you will have a new model that is independent of the legacy design.

[KenFarley]

There's no easy way I know of. What I've done in similar situations depends on the complexity of the model I'm trying to "fix".

Approach 1

What I do if the model is not that complex, or even if it is very complex but crippled by unstable sections, has any other corruption, etc. is to just remodel the thing, starting with an empty model. If possible I'll load up two sessions of Creo and use one to look at the old garbage model, and the other to make the nice clean new model. I've also used an assembly of the old and the new to make sure as I go along that the geometry is the same, etc.

This might seem like the longest way to get the improved model, but often it isn't, mostly because I am not being forced to deal with bad features or other things I can't trust.

Approach 2

If the problem is a bunch of features that really don't do anything, or become redundant, or maybe I want to replace a poorly modeled three features with a single better one, I take a different approach. I'll turn on visibility of suppressed features in the model tree. Then I will suppress a feature I want to get rid of, and see what other feature(s) it affects. I then go into the affected feature(s), if I'm hoping to keep them, and fix any references that connect them to the "bad" feature. Once all the dependencies on the "bad" feature have been corrected, I suppress it one last time, and if all is well, I then delete it. I do this for all the features I want to eliminate. It's somewhat tedious, but works great if there are only a few bad features I want to get rid of - it's much better than remodeling the whole thing.

Approach 3

This is if I've given up on trying to retain any of the bad features and I just don't care about what they kill with them. I resequence the features as much as possible to get all the bad features at or near the end of the model tree. Then I just delete them, and take the consequences in terms of collateral damage. Then I rebuild new features with the "proper" techniques I'm trying to implement.

So, no quick method, but then again I'd rather put the time in to fix a model than be haunted by my past bad geometry creation. Do keep in mind though that you can save sketches that were used for features to their own *.sec.* files and then pull them into another file. In this way you can save yourself from recreating the geometry for features you like.

[Dale_Rosema]

Similar to Approach #2 above, I will suspend the features that are affected by the culprits and then delete the bad features. Then progressing down the tree, I redo the suspended features.

[tbraxton]

@KenFarley addresses the question of it depends on what you are starting with and what your deliverable requirements are. 

Another tool that I use extensively in this context is the copy/paste functionality. Creo supports copying features from one model and pasting them into another model using paste special (Ctrl+Shift+V). This will allow you to salvage work in the "bad" model if there are some features suitable for re-use. You have to assess this in the context of time required to copy vs. re build of course.

This scenario is more frequent than you might think as there is no shortage of unmanageable models in existence. 

My most recent rebuild was one where I rebuilt from scratch and did not reuse anything from the reference model. A client provided a part with 2000 features worth of convoluted "hack and whack" features in a model that took so long to regenerate that I was astonished that anyone was actually working with it. The objective was to modify the design to make new production tooling for a design variant from the reference part. I immediately determined that starting over was the path of least resistance. This model now occupies a top spot in the hall of shame as an example of what not to do with Creo. 

When I was done rebuilding this model there were 386 features and it of course regenerated in a small fraction of the time relative to the reference model. 

[KenFarley]

Oh boy, this brings back memories. Had a similar situation with a multi-thousand feature part. Lots and lots of what I like to call "electronic JB weld" features, where they'd fill in no longer wanted holes or cutouts, then create new ones. All with protrusions up to complex surfaces.

I was working as a "hired gun" and didn't feel comfortable re-doing the model, so I hobbled along and eventually got what I needed, but it was agony. And I still feel bad about it. Kind of like I let a criminal get away with a horrible crime. Which is kind of true.

[Dale_Rosema]

Sounds like my predecessor twice removed.  🙂

[tbraxton]

There are plenty of users out there that are quite adept at applying the Pro/Bondo module to models to cover up their lack of competence within Creo. Most orgs do not track the cost of poor quality associated with this type of thing and it lives on. 

Test the knowledge of anyone who claims to be proficient with Creo prior to hiring, it can be done in 30 min or less verbally on the phone. If they don't pass that screen then assume they know nothing (or learned bad practices) about Creo.

[StephenW]

The steps presented by Ken are my most used methods. 

If you don't want a modifiable model as the deliverable, there is also the collapse functionality under the model tab, then the drop down arrow for editing. It is useful in some cases.