Replace Component Drawing view problems

[Bishbosh]

NX7.5
What is the procedure when after 'Replace Component' in the model file to update an existing Drawing.
Views have been added using Base View - Add Part, the problem is, the existing views are referencing part numbers that have changed, and after the model update, the Drawing views are empty.

 

[JohnRBaker]

Is there a reason WHY you created Drawing views using the 'Add Part' approach? I mean, did you really want to include parts from other files in your Drawing? Under normal conditions, you should create your Drawing views from the Work Part, which is the default when creating a Drawing.

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.

 

[Bishbosh]

Sorry, I meant 'Part' at the top of the Base View dialogue window to specify only one Part of the assembly to be visible in the view.
My new assembly has different part numbers to the ones used previously.

 

[JohnRBaker]

If your goal is to have a Drawing view showing only ONE of the Components of the Assembly that you're creating the drawing of, go ahead and add a normal view of the Assembly and then go to...

Assemblies -> Context Control -> Hide Components in View...

...and select ALL the Components. Now don't use the drag cursor method since this will miss any Components hidden by others. It's better to pick the 'Select All' icon on the Selection Bar (if it's not enabled just hit 'Ctrl+A'). Now if you can see the Component that you wish to keep in ANY view, simply de-select it by holding down the shift key and selecting the Component-of-interest. Now it doesn't have to be selected in the view that you're wishing to create, the Component can be selected in ANY view on the Drawing. Once it's selected, press MB2 and then select the View that you're creating and then hit OK. Now do a View Update and you should be good to go. If the orientation of the view was not what you wanted, you can always edit the view and using the 'Orient View Tool' to get the Component oriented properly.

Now if it's not convenient to de-select the Component-of-interest when hiding the Components go ahead and hide them ALL and then go to...

Assemblies -> Context Control -> Show Components in View...

...and select the view that you just hid all the Components in, press MB2 and then from the list in the dialog or from the Assembly Navigator, select the Component-of-interest and hit OK. Now as mentioned above, do a View Update and then reorient if needed.

Anyway, this in one way to go that will avoid using a separate 'Part View' and you should avoid the Replace Component problems.

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.