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Simplify a Assembly into a part

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Simplify a Assembly into a part

Hello All,

Just wondering how people go about creating simplified models of sub assemblies.

The specific thing I am working on is an assembly with several different bearings. While I want to keep the bearings in the assembly and it is nice they look like bearings when sectioned etc I would like to to simplify them. By simplify I mean ideally turn them into a single part. The bearings currently are as downloaded from the bearing supplier and each one has a dozen different parts. For this project I want to keep everything in a single folder and having lots of bearing parts is making it more difficult to see the other parts. Also I have to email assemblies and it would be better if the bearing was then just one part, instead of several.

I could remodel the, but this seems time consuming and unnecessary.

I also could Shrinkwrap them, but this creates external surfaces only.  

Any recommendations would be appreciated.

Thank you.

17 REPLIES 17

Re: Simplify a Assembly into a part

Shrinkwrap is used to create solid geometry and depending on the quality level you choose, the part can be identical, internally and externally, to the original model. It is definitely the easiest method. If the option isnt' available, there is some problem with the original model such as it contains surface models or has some sort of geometry that can't be converted.

shrink.jpg

Other options are external merge/inheritance (may be an option not available to all), merge (creates a reference to the original model and a merge part in the original model) and using a step export and re-import with the option to make as a single part (there is an option to do this but it eludes my memory at the moment).


Steve Williams
Pro/E Version 15/16 (Circa 1995/1996)

Re: Simplify a Assembly into a part

Hello Stephen, thanks for the quick response. Using shrinkwrap it is always fills the internals for me. I am selecting the Merged Solid option already.

I have tried putting the level to 10, and it makes no difference. Unless I unclick all the special handling boxes it justs gives me a single cylinder with rounded edges (So loses all the shield and race details.

Thanks

Re: Simplify a Assembly into a part

Can you upload the vendor bearing?


Steve Williams
Pro/E Version 15/16 (Circa 1995/1996)

Re: Simplify a Assembly into a part

The particular file I am working on currently is attached. But I am also interested more generally in what people do with their own sub assemblies.

Thanks for any help 

Re: Simplify a Assembly into a part

I exported your assy as a STEP and re-imported as a prt.  Creo will recogize it as an assy, you'll need to check part in the import dialog:

Capture.JPG

The only hiccup was that it only brought in one of the balls, instead of all 16.  I've attached my part here.

--
Doug Schaefer | Experienced Mechanical Design Engineer
LinkedIn

Re: Simplify a Assembly into a part

It's CREO 3 models. Unfortunately I am unable to read Creo 3 models at this time. I was supposed to already be testing it but haven't taken the time to install it yet.


Steve Williams
Pro/E Version 15/16 (Circa 1995/1996)

Re: Simplify a Assembly into a part

The problem with importing step file assemblies as parts is Creo will simply "pile" all the different parts on top of each other (based on the coordinate system).  To fix this, set intf3d_in_as_part to yes in your config.pro file before attempting to import the file.  Now assemblies can be brought in as single parts but still maintain the proper spatial relationships between the different components.

Re: Simplify a Assembly into a part

Here is the bearing following your process but with that config option enabled.  (Creo 3.0)

Re: Simplify a Assembly into a part

Interesting.  Unfortunately, that option also make importing as a part the default, which I definately don't want/

Also, when importing with that option set, Creo created a bunch of extra layers, with the solid geom on every layer.  But the balls were all there.  Without it set, no extra layers but only the two balls.  I tried in both Creo 2 & Creo 3 with the same results.

--
Doug Schaefer | Experienced Mechanical Design Engineer
LinkedIn
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