REPLACE COMPONENTS IN NX 10 1

[KUNAYALA]

Hello¡

I´m working with NX 10 with a lot of drawings of a very similar 3d models. When I try to replace component in a existing drawing
I find that the application doesn´t work properly...I am not able to pick the component to be replaced.
Anybody knows if this application can be used in this NX vERSION?

Thanks in advance for all your support¡


Sergio G.

Industrial designeer

 

[niedzviedz]

Hello,

What version of MR and MP You are using? The last one is MR3 MP19 for NX 10. Could You provide some example of drawing, picture or some movie what You are doing strep by step etc. Because I used NX 10 for long time and never experienced that NX can't replace component in drawing. That's why I think You're doing something wrong.

With best regards
Michael

 

[jerry1423]

Yes, replace component, should work properly in NX10.
Are you working in Modeling (not Gateway) with Assemblies ?

Jerry J.
UGV5-NX11

 

[KUNAYALA]

Hello,
I work with assemblies, but when I make the drawings and I want to replace the 3d component in the drawings along aplication Asembly--> Replace component ( within drawing environment).
Unfortunately when I run the application, it doesn´t allow me to pick any component….. I attach an image

Thanks a lot for all you replys and support¡

Sergio G.

Industrial engineer

 

[NutAce]

A picture says a thousand words....

Your component is not really in the Drawing "Assembly" structure. You used the View from model to place the view.

Here you can see the difference. The top Component is added as a real component to the Drawing Structure. (this is done automatically by NX when you create a new drawing from a 3D model)
The bottom "component" is added as a view later on (the difference is in the icon). It is not really there it is just referenced. If you look in the properties you can see that it is set to reference only.
Therefor you can't replace it. There is nothing to replace.

If you want to be able to replace the components in the future, then you first need to add them (like in an assembly) and then afterwards create the views for it.

I just noticed something... Before NX12 you were able to remove that "For Reference Only" property. Apparently this is no longer possible?



Ronald van den Broek
Senior Application Engineer
Winterthur Gas & Diesel Ltd
NX9 / TC10.1.2

Building new PLM environment from Scratch using NX12 / TC11

 

[KUNAYALA]

Hello Ronald,

Thank you for your reply but I am not sure to understand you...

I will repeat the issue with a new picture; My design has a couple of a very similar parts ( part 1 & part 2)
and I must create a single drawing detail of each one I order to be able to launch and mechanised it…

In an previous NX Versions as NX6 to NX8: I made a drawing of a part 1 for instance and once it was finished and
I wanted to create a drawing for a part 2 ( I repeat, avery similar part) starting from a drawing of part 1, it was
very easy through command Replace component in a view...
I have realized that this way to handle similar cases is not functional with NX 10 version....
According your words... Must I foresee to create a component with a similar parts in order to be able to replace them
in drawings?


I appreciate your support in advance!


Sergio G.

Industrial engineer

 

[jerry1423]

RMC (right mouse click) on the model file in the ANT of your drawing file -> then select Replace Component
If you are unable to select that model file you may not have your filter set correctly. In this situation you either want it set
to Component (shown below) or, No Selection Filter

{Added} Actually the filer that I mentioned does not seem to be a factor here.
If you cannot select the model file then there may be an issue with Read/Write permissions to that file.



Jerry J.
UGV5-NX11

 

[KUNAYALA]

Application "Replace component" does not allow me to select the component to be replaced...

 

[jerry1423]

In your Assembly Navigator
What happens when you touch (with your mouse pointer) UTIL_ENTRADA_SFF_825_519_GR04_002 ?

Jerry J.
UGV5-NX11

 

[cowski]

The yellow cube icon denotes an assembly component; the yellow cube over a drawing page indicates a drafting component. Drafting components do now show up in the graphics window when you switch to the modeling application nor do they show up in a parts list on the drawing. These views are mainly used for reference. In older versions of NX, you could use the "replace component" command on these views. This was intentionally removed in NX 9; no equivalent command has been added to enable what seems to be a common need.

There is a bit of a trick to "replace" these drafting components, but dimensions and annotations in the view will likely lose their associativity. In the drawing, add a base view from the part that you want to see in your drawing, right click the existing view that you want to replace, go to settings and expand the "inherit" section at the bottom (if needed), change the settings source to "selected object" and select the newly added view of the part you want to use. The existing view will update to show the same part. Delete the newly added view and reattach dimensions and annotations as necessary in the existing view.

www.nxjournaling.com

 

[KUNAYALA]

Great reply Cowski¡¡

Unfortunately you are right and the most of annotations get lost… I find NX must fix this issue because in my sector this command isusually used.
Other programsd as Catia V5 has this point fixed sucessfully....

Anyway I apreciate all the suppport¡