Exporting Promoted Bodies 1

[Manley23]

Hello Everyone,

Recently I had a very huge assembly which needed to be scaled down, so I promoted all the bodies in the assembly and scaled it down to the required value. This created additional feature of promote bodies in the part navigator. Now when I try exporting this file as STEP it does not export the promoted bodies. So the output is basically the unscaled body.

I do not understand why this is happening. Can somebody educate me on this? I actually want to know how to scale huge assemblies in one command or as less commands as possible. I do not want to scale individual components. Please provide suggestions on exporting promoted bodies as well. All help will be appreciated.


Thanks in advance.

 

[aluminum2]

Not sure why it wouldn't work, but have you tried to wavelink the bodies instead?

 

[Manley23]

No I have not used wavelink bodies. I am new to UG NX (using NX 7.5). Can you please explain little more in detail as to how it is done. The assembly I am dealing with is a huge assembly with some hundred parts and few sub-assemblies. Is there any quick way of doing it. Please suggest. Do I need to wavelink body at the sub-assembly level first and then at the main assembly level?

 

[cowski]

Recently I had a very huge assembly which needed to be scaled down...

Is this something that you will be doing often or is this a "one-off" type of operation?

If this is something that you will only be doing occasionally, I'd suggest exporting the assembly to a parasolid file then start a new NX part file and import the parasolid file. You'll have a bunch of "body" objects that you can scale as desired and export to a STEP file. The upside is: it will be independent of your assembly, it won't affect your current assembly in any way. The downside is: it will be independent of your asssembly, if/when the assembly changes you will need to repeat the entire process.

www.nxjournaling.com

 

[Manley23]

Hello Cowski,

This I generally have to do occasionally. But I tried with parasolid option but I do not know why I was unable to open the STEP file generated. Also if I use the parasolid feature, after converting it into STEP and opening in a different CAD software I will not be able to open individual parts. Please help.

 

[cowski]

Yes, you will lose the assembly structure by going the parasolid route; but I think that would also be true of the promote body or wave link methods as well.

Off the top of my head, the only way I can see to keep the assembly structure would be to scale down each component body in its corresponding part file (go into each part, create an extract body, scale down the extract body, and create a new reference set for the scaled extract body). Switch back to the assembly (or subassembly), and change the reference set used to the one holding the new scaled body. However, all constraints will be lost (or more likely will not be correct for the scaled bodies) and you will most likely have to re-assemble your components. Not fun, even for an occasional operation.

www.nxjournaling.com

 

[Manley23]

Thanks Cowski. Yes it is a tedious process. Anyways thank you for the tips and suggestions.

 

[Toost]

I gave it a spin, it works fine for me.

when exporting, The results will be more "as expected" if you use the option "existing Part" instead of "Displayed Part".
In the Data to export, what options did you turn On ?

regards,
Tomas

 

[Manley23]

Hello Thomas,

While exporting I just checked the box against "Solids" to reduce the file size. Am I going wrong here? And I actually export the displayed part. Do you want me to export using the "Existing Part" option?

Thanks.

 

[Toost]

When you export using the "displayed part" option, you have the option to select things for the export ( which you don't have when using the "Existing part" option.)
This selection step have a tendency to screw things up for the users i support, either they do not select the things they think , or there is something else that makes the exported result different from what the user expected.
The "Existing part" on the other hand is more as expected. "what's in the saved part will be exported."

In my test i had "Solids" and "Product data" both ON when i exported.

Regards,
Tomas

 

[Manley23]

Thanks Tomas. I'll try this.