We have a number of components that were created by downloading a STEP or Solidworks file from the vendor and then importing them into our Creo start part to set our parameters. Most of these are pipe fittings and we have created an extrude to 'blank' the threads that they were originally modelled with. Then we added ports and coordinate systems to use with piping.
I modeled one fitting from scratch and did the ports and all. When I looked in ModelCheck for File Size, my model was about 30% of the imported model size.
Does file size have an impact on regeneration time? We might have close to 100 imported fittings in some of these larger files.
I think an extrude to blank the threads and such will probably greatly improve rendering (i.e. hidden line removed views on drawings or as the view state) but might actually increase regeneration time. Creo's still got to interpret all those imported surfaces and build a solid from them before your thread erasing feature can be added.
Anecdotally speaking, I've noticed that folks in my company that use lots of imported models from catalogs and such have assemblies that take an inordinate amount of time to load in. I think it's all the surfaces in the imports and the solidification (if it's able to) take a long time to regenerate when they're being loaded in. There's probably a good amount of tangency and gap checking going on, etc.
My tendency, unless it's something far too complicated, is to build a native Creo model of things and use that, with all the proper parameters and such to reflect the eventual purchasing source. Assemblies I've used this philosophy on, though large, seem to load in much faster.
From regeneration tests I've done, I've have to say yes. It's also graphics dependent (some small but complicated features taking more regen time than larger simpler features). I've got settings to speed up the graphics by minimizing detail when you're zoomed out, forget the names offhand.
Also, I wouldn't ADD complexity to the model by adding a solid feature to cover up modeled helical threads. The geometry is still buried in the model taking up space and regen time. I have no idea why modelers for McMaster-Carr for instance (Ugh! JUNK downloads...) actually model (badly) helical threads. I remember they didn't even used to be helical, just SLANTED, so that when you looked at them from one side, they looked like right-hand threads, and if you looked at them from the other side, they looked like left-hand threads! Not even close to correct, and just taking up space. So, what I do whenever I import a STEP model with helical threads (unless I absolutely need them for some really odd reason - never the case yet), I go into Import Data Doctor and manually delete all those surfaces. Then I add the correct major diameter as a surface (for external threads, minor diameter for internal), merge the quilt, then make it a solid. I usually manually add the correct cosmetic thread to it to finish it off. Easy, simple, clean, and takes up a TON less space and graphics regenerations time. I'd suggest going into ALL your start parts and doing this, and do the same for every imported file you use that has helical (or helical-ish) threads. I think you'll find that, especially if many of these are used in a large assembly, that you'll considerably shorten your regen time. I think you've already proved the worth of what I'm talking about.
Best of luck!
I agree that the best approach is to delete any geometry from the import data using the IDD tools. If you do not want to manually manipulate those data sets then you can try importing the data into Creo and then exporting it as a Creo neutral format. In some cases this may result in decreased regen times but I think there is an even better solution that does not require geometry manipulation and will still speed things up for load and regen.
Save all of your "library" parts with all features set to read only. I have used this to dramatically reduce load and regen on assemblies with over 1000 components.
Good point on the "read only" features. You can also set up Simplified reps to "Graphics Rep" (or other lightweight setting) for all library parts. If it's a graphics issue, as it is many times in an assembly with many fasteners, making features read-only won't help though, the best thing is to get rid of unwanted geometry so the graphics card doesn't have to crunch numbers. Another reason why I've turned my "prehighlight" off and use the Olde School "Query-Select" setting.