saving drawing file with assy parts

[BABUGOUDA]

Hello,
I have a Drawing file and assembly file which is used for creation of the drawing in NX 8,5.
Now i have two questions
option-1.once the drawing is complete i need to SAVE AS my drawing file along with children parts and assy file every thing to another output directory. so that the end user after receiving the folder will get the proper links with the drawing file

option-2 i need to SAVE AS the drawing file to another directory and just move the children parts to folder without saving assy and child parts (like send to direcory in catia V5)so that the end user after receiving the folder will get the proper links with the drawing file

What i feel is with these above methods, it is sure that no links will be broken with drawing file.
if any body knows good equivalent methods like in CATIA V5 --1. save management 2. Send to direcory.. please share...

I am using UGNX8.5

Thx
Pat...

 

[aluminum2]

It sounds to me like you want to give the assembly files to another person outside your network. If that is the case then the easiest way would be just to copy and paste all the files (in windows) and place them in a single folder. Then in UG under file->options_> assembly load options choose load from folder. Then open the file you want.

If its internal on a network and you want to do a save as then you should look into cloning. There is a youtube video on it.

 

[JohnRBaker]

If you're really looking to provide all of the content of an assembly to some external person, I would suggest that you look into using the 'UGZIP' utility to assist you in that task. For more information about this, please review this recent Eng-Tips thread:

http://www.eng-tips.com/viewthread.cfm?qid=345894

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.

 

[SvenBom]

Have you tried Clone Assembly?
Just go to menu Assemblies->Cloning->Create Clone Assembly. There you can define, if you want to copy/clone the whole assembly with all the parts into a new directory or just the assembly file.
I have just done a test with the drawing of an assembly:
[ul]
[li]I have cloned all the parts and the assemblies and the drawing to a new directory. I have clicked the Add Assembly button and selected the prt file for the drawings. All the parts in this assembly are added automatically. You don't have to click on Add Part button. I have also defined, that all the parts and assemblies will get a new name. Every prt file receieved a prefix like 'clone-'. This was done in under the Naming tab with Define Namening Rule option. In Nameing tab, you also have the option for the output directory. That is directory, where all the asseblies and parts will be save.[/li]
[li]Then in second test, I have cloned just the drawing. In Create Clone Assembly, in Main tab, with Add Assembly button I have selected the prt file for the drawing. In Main tab, there is also Deafult Clone action, which is set to Clone. I have clikced here on the Exception button. Here, I have selected all the listed parts, except the drawing part. To all those parts, I have set new action, which was Retain. That means, that only the drawing part will be cloned/copied to the new location. The actuall assembly and all the parts will not be copied. But, the drawing will still have the link to this assembly. So, if the assembly is changed, the drawing will change. Then in Naming tab, I have selected the deafult name for cloned drawing and the output directory. And that's it. The drawing was copied and it has link to the assembly.[/li]
[/ul]

To use this command, you have to be in Modeling or Gateway environment not in drafting. Actually, you don't have to open any file. If you have Assemblies menu on, when you open NX it is enough. You can start cloning the assemblies. But, if you are in drafting, then you have to switch first to Modeling or Gateway and you will have this option.

If you need more detailed description or a movie, let me know.

 

[BABUGOUDA]

Thank you very much SvenBom.
my question is solved with your 1st test method as it copied all the parts to new directory .here all the file details shows that they are modified( recent time and date).
my 2nd requirement is i don't want to save all the data except the drawing to new directory but need to move( like cut paste). so that customer understands that i have not saved his parts and only worked on drawing file.

UGNX

THX
pat..

 

[SvenBom]

For your 2nd requirement, I am not sure, if I understand it corectly. My guess would be to use one of the following:
Save Workpart Only: it saves just the drawing (active work part) only. No other parts in the assembly will be saved. But it will not ask you for the directory, in which to save. It will just save the drawing.
Save As: It will save only the work part, which is drawing, and not the assembly with its parts. I have just tried this. I have created a drawing for an assembly and used Save As. I have saved it to another directory. Then I have checked the Information->Part->Part History. If I checked the part history for the assembly, I could see, that the last save was done some month ago.

 

[looslib]

If you are creating the drawing only from customer supplied models and assemblies, put all of the customer files in a dedicated directory and set them to read-only. Then create your drawing in that same directory. NX will recognize that the models are rear-only and not let you save them, but you can save your drawing. When completed, package the directory and send back to the customer. UGZip will also work for this, too.



"Wildfires are dangerous, hard to control, and economically catastrophic."

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