Converting Assembly to Part

[Phil_K]

Version Creo 9 

Good Morning. I received this as a step file which opens as a assembly. I am making one of the horizontal pieces about 17" longer. Because it is an assembly with no constraints already built in, I have to move and constrain all pieces next to the 17" lengthened pipe. Is there a way to just save this as a multibody part and make the change so that everything moves together?
I have tried file and save as to see if I could just output it as a part but that doesn't seem like an option. I am used to Solidworks where everything is easier. Thanks in advance

[Chris3]

You can import it as a part using the hidden config option 

intf3d_in_as_part YES

Put this line in your config.pro. Since it is hidden it will not show up if you search for it.

This will create a single body part. Multibody assembly to part is coming in a future release.

I am not sure any of this is exactly what you want though. 

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@Phil_K wrote:

 make the change so that everything moves together?

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In order for there to be relative changes there needs to be constraints or parametric relationships that tie the geometry together.

Sounds to me like what you want to do is open it as a part and then use flexible modeling to make it longer. You can do that with the config option above and the flexible modeling tab.

[Phil_K]

Thank you for replying! Yes, that is what I want to do. 
Can you give me more details on the hidden config options? How do view/change them? In that area I can only see:

[MartinHanak]

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@Phil_K wrote:

Thank you for replying! Yes, that is what I want to do. 
Can you give me more details on the hidden config options? How do view/change them? In that area I can only see:

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Hi,

open config.pro in Notepad/Notepad++ and type the option manually ... see below. Save file and restart Creo.

[kdirth · Accepted solution]

In the configuration editor you can select Add... and enter the config and setting.  For hidden configs you will have to type in all of the text for the name and value as they will not show up.

[Phil_K]

Success! I wasn't able to get it in the notepad but I may have not typed it correctly. Once I added it in the configuration editor, it accepted it.
Thank you everyone, this is a big help! I do most of my stuff in part files. 
Follow up question, If I arrange a few items in an assembly, can I bring it right to a part file? 
I could save it as a step and open it in part using the above method, but can I directly export it from Creo assembly to Creo part?

[MartinHanak]

Simple answer is no. You cannot save assembly as part.

[Phil_K]

Thats a bummer... thanks anyways!

[Chris3]

Yes you can. You can use inheritance features to bring them in. Model Tab - > Get Data -> Merge/Inheritance

You can also use publish / copy geometry to publish the bodies from individual parts and bring them in.

This may not work exactly how you are used to it working and leads to large geometries with not great performance but it can be done. As I mentioned before, PTC is working on making it better / easier.

[Chris3]

If you are using Creo 11 there is a new way to do this with shrink wraps. See link below:

https://support.ptc.com/help/creo/creo_pma/r11.0/usascii/index.html#page/whats_new_pma/asm_multibody_support_in_shrinkwrap_feature.html 

[Phil_K]

Thanks Chris3, I am familiar with the shrinkwrap and copy geometry way, somewhat. In many cases saving to a step and importing as a part will actually be faster and more accurate. 
I hope they do fix it in future versions. The company I work for only uses Creo and I'm really not a fan because of hurdles like this.
I'm still getting the hang of it though so I can't hate on it too much. 

[StephenW]

Just about every method of saving an assembly to a part (shrinkwrap, merge, export/import, etc) has its quirks and issues. You will need to find the one that works best for your models. And sometimes you will need adjust based on the specific model.