bodies to assembly

[jwmolddesign]

I am an I-deas user trying to learn NX8.

I have imported a step file with no assembly structure into NX. The file contains about 650 solid bodies. I need to get these bodies into a structured assembly so different groups of components can be turned off and on in an organized manor. Basically what I think I need is a way to convert the bodies into NX parts. Then I can add the parts to an assembly. I don’t want to take the time to name every nut and bolt in the entire file and export as a part.

I-deas would import these bodies as parts and then I could move the parts to assemblies.

I use another software (Cimatron) where I have a switch on import which will place all the separate parts into an assembly. The parts are named Part1, Part2 and so on but then I create some sub-assemblies and move the parts to make an organize structure.

Any help would be appreciated. Thanks in advance.

 

[JohnRBaker]

From what system was the model imported and which Translator did you use?

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
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[jwmolddesign]

The step file was written from NX7.5 I imported the file into NX8. As for the translator, I created a new NX session and went File > Import > STEP203

 

[eex23]

Re-export already opened structure to parasolid: File->Export->Parasolid. Save it. After that you will get quite large one file XXX.x_t. Then just open this file (not import) with NX. And as a result you will get an assembly with components and not solid bodies.

 

[Toost]

Step export from NX can be done with or without assembly structure, ( - I assume that the person that step exported the parts from NX for re-import into NX wanted to hide something and therefore used STEP ? ... )
- If you can, get a copy of the original NX files. If that is impossible , You could ask the exporter to re export Step with assembly structure.

Likewise, you can flatten an assembly on step import if you desire that.

If you are stuck with the case 650 bodies and a single partfile and want to convert that into an assembly, make sure that the assemblies application is=on, then Assemblies - Components - Create new Component - enter name+ OK - Select the body to be exported into the new component file ( have the "delete original objects"=on) + OK, note the "blink" of that body, the body has been transferred into the new component partfile but keeps the position on screen. Open Assembly navigator to verify.
( Note that if the selected body should repeat in the assembly, you should delete the remaining copies and manually place components there as soon as the first is completed. - There is no way NX "understands" that "n" identical bodies should be replaced by one component.)

Since the assembly is 650 bodies, somebody can probably aid in automating the above with a journal. ( -Cowski... ?)

Regards,
Tomas

 

[jwmolddesign]

Thanks eex23, that’s exactly what I needed. I would have never thought the parasolid open would act differently than the parasolid import.

I would still rather have a switch on the import to separate the bodies into parts. My fear is since I deal with a lot of junky data I am going to end up with some parts in my assembly that should be stitched together into one part. But that is a worry for another day. Thanks again.

 

[JohnRBaker]

With 'Import', we're performing the literal meaning of the word; it's going to IMPORT the contents of the file into either an existing file or a new file, but it's doing exactly as it says it's going to do, IMPORT the contents into a SINGLE file. However, doing an 'Open' implies that it's not 'importing' anything into another file, but rather will attempt to OPEN the contents of the file and if it's organized as multiple parts, i.e. an assembly, then that's what you'll get.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.