how can I seperate the the drawing file from inside the 3D part file 2

[sam5a1]

We use the master model concept for all our models and drawings. But, we have a lot of 2D I-deas drawings that we are going to use and need to bring into NX. we are looking at using the CMM on on these drawings after they are migrated into Teamcenter. The issue is that when an I-deas drawing is imported into NX or converted to NX through the CMM, it puts the drawing in the model file. How can I convert these into the master model style, or better still, how can I bring I-deas drawings into NX as the master model style?

 

[JohnRBaker]

In essence what you're asking to do is to convert a 'Part' file into a 'Drawing' file which is actually an Assembly where the 'Part' is now a Component of that Assembly. This is true whether the 'Part' file was a single piece part or an assembly itself, for your purposes, if you can just get the 'Part' to be a Component of the Assembly in the 'Drawing' file you've got what you want, correct?

Anyway, the function that you're looking for is...

Assemblies -> Components -> Create New Component...

...where, while in the current part file, you will select all of the geometry (but not the dimensions, notes or any other anotation that you wish to remain with the 'Drawing' file), or in the case of an Assembly, all of the Components, and create a NEW part file which will now contain the selected geometry or those components. And as you're doing this, that new part file automatically becomes a 'Component' in the Drawing file. And everything should remain pretty much as you see it, including dimensions still associated with the correct geometry and the view still showing the correct items etc.

I would suggest that you review the NX Help files for an explanation as to how to use this function as well as comments about how and what objects can be moved from the what will now be the top-level part to the new part and how and what relationships are maintained.

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.

 

[PSI-CAD]

Hi John,

I never tried this method, because I always use master model approach. But many of my customers will migrate to Teamcenter and they have a lot of drawing inside the 3D part.

So I am trying to day and with my first example all my dimensions become no associative.

Any Idea ? have a look at the jpeg file

I am using NX8.5

TIA


Regards
Didier Psaltopoulos

http://www.psi-cad.com

 

[kapmnit123]

Hi DidierPSICAD,
Try this.
(1) Open the part (where the drafting resides) and then open the sheet.
(2) Go to FILE-EXPORT-PART and choose Select NEW PART then select DRAWING SELECTION (which prompts you to select the sheet)....Select it and press OK.
(3) Now NX will ask you (prompting automatically) "if you want your part to be a component of a master model"...... say YES
(4) Now when you open your NEW PART (master model) you will find that the drawing now resides at the assembly level (master model).

the only catch is that you need to go back to the original model and delete the drawing (unluckily this creates two copies of drawing...one in the original child part and one in the master model so delte the one in the child part)...
But it always retains it's associativity ....
I know it's sort of a manual effort but can't find any other method for it.

Do let me how it works...

Best Regards
Kapil Sharma

 

[PSI-CAD]

Hi Kapil

Thanks a lot


Regards
Didier Psaltopoulos

http://www.psi-cad.com

 

[sam5a1]

Thanks for the These work for the items that have models associated to the drawings and for making the Master Model within the item. Unfortunatly I also have a lot of drawing that I need to get into the Master Modeler as specifications, see the jpeg for a better explanation. We are migrating I-deas into Teamcenter (already have NX there) and I need to make the I-deas unassociated drawings as a specification to a master.


Scott Martin
NX 7.5.4.4
Tc 8.3.2
I-deas 6m2