Import an view of an assembly into a component drawing

[dumboplume74]

Hello !
I have an assembly file called ASSEMBLY which contains the components 1 and 2.
In the drawing of component 1 , I would like to import a view from the ASSEMBLY file.

How to do if I want to be associative ?

Best regards.

 

[SvenBom]

Which version of Nx do you use?
If you have created a drawing for a component1, you have to do this:
1. click on Base View command (Insert/View menu)
2. in Base View dialog box, open Part section (first section on the top of the dialog box)
3. in this section, click on Open command and select the assembly, for which you want to create a drawing view

The reason I asked for the NX version is, because in some older versions, this procedure was slightly different. What I have described is for NX7.5 and later. I some older versions, there was a separate command for this. Base View was for creating views from the first part, you've placed on the drawing. And then there was a PartView command or something like that. With this command, you've selected new part and placed it on the drawing.
So, if you don't find the Part section in BaseView command, then search for PartView or something similar.

 

[dumboplume74]

Hello SvenBom !
thanks for your answer !

I'm working with NX 7.5.3.3

The process you are mentioning is working in the case:
I want to import a view of the file 1 into the file ASSEMBLY.
But my today issue is the opposit process :
I want to import a view of the ASSEMBLY into the file 1.

It seems that there is a crcular problem for UniGraphics.

A solution proposed by one of my collegue is to seperate the model 1 from its drawing. So I have created a file 1-DR just for the drawing.
At that moment , the process you describe is working but unfortunately we are in a laboratory with 5 designers and the official rule is not to separate model and drawing.

If you have any over idea , I am still interested !

Bye

 

[JohnRBaker]

This works fine in NX 7.5 (as described by SvenBom). I created the Drawing shown below where the Drawing is of the 'Handle' of the 'Valve Assembly' as seen in the view of the Assembly that I added as an additional 'Base View'. This is basic functionality and there are no 'circular' issues.

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.

 

[dumboplume74]

Hello John !
what you are showing is exactly what I need.

Do you have drawing separated from the model as described in my previous answer ?

Best regards.

 

[JohnRBaker]

This is a 'Master Model' drawing where the model of the 'Handle' is in one part file and this Drawing is in another part file referencing the 'Handle' (shown as the 'arm' in the image below) as well as the Valve Assembly which is in ANOTHER part file.

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.

 

[cowski]

It should also be noted that the master model method (model in its own file: drawing, CAM, FEA, etc in their own individual files) is the recommended way to use NX.

www.nxjournaling.com

 

[dumboplume74]

OK, John and cowski,
by using 2 separate files (1 for the model + 1 for the drawing ) , your process works perfectly.

Unfortunately, in my laboratory (5 designers) , the rule is to have model and drawing in the same file. The only reason is just because we didn't get investment for the software to manage revision. We've tried to manage revision manualy but it was too complicated.

Thanks for your help !
Good bye.

 

[SDETERS]

Would using assembly arrangements get you the same thing? So you would have an assembly with part 1 and part 2. In one arrangement you have just part 1 with part 2 supressed. Then you would have another arrangement where both parts 1 and 2 are not suppressed. So your drawing would reference a master assembly. So when you put your Base views into your drawing you will use different arragnements to define your base view from. There may be a work around for existing parts-drawing you want your assembly into. But to start new assemblies this may help?