REPLACE COMPONENT IN DRAWING

[Javiduc]

I have created a drawing file using master model approach. Then I created some views; base view and then a section view from base view. I have renamed the part in windows environment and then replaced the part in the NX assembly environment. Then, the base view is linked to the "new" part and can be updated, but the section view is still linked to the old non-existing part and can't be updated. Am I doing something wrong? Can I change links to other model files in a different way? Thank you

 

[NutAce]

There is no way to change the reference of a view...It is a bit strange though that the Section view won't update anymore...
It's reference should be the Base view.
Where did you find out it is still referenced to the old part?

Ronald van den Broek
Senior Application Engineer
Winterthur Gas & Diesel Ltd
NX9 / TC10.1.2
HPZ420 Intel(R) Xeon(R) CPU E5-1620 0 @ 3.60GHz, 32 Gb Win7 64B
Nvidea Quadro4000 2048MB DDR5

HP Zbook15
Intel(R) Core(TM) i7-4800MQ
CPU @ 2.70 GHz Win7 64b
Nvidia K1100M 2048 MB DDR5

 

[ewh]

Have you tried editing the section line and reattaching it to the same point as the original?

"Know the rules well, so you can break them effectively."
-Dalai Lama XIV

 

[Javiduc]

I found that it was still referenced to the old part because when trying to update, an error message appeared telling me that was impossible to update because file was not available (I don' rememeber the exacts words).

I have tried to do it again with newly created files and it had worked both with some point of the section line attached to a point in the base view and without attach it to any point and now it has worked properly in both ways. Something wrong must had happened with the previous test, it is a pity that I erased the views in order to create then again. But I am happy I can change links in drawing files now, I think it is very useful.

Thank you both for answering.

 

[cowski]

I have renamed the part in windows environment...

This will break links in your file(s). To maintain the links, load all the affected files (model, drawing, assembly, any files that wave link geometry from this file, etc) in the same NX session and perform a "save-as" on the model file.

www.nxjournaling.com

 

[Javiduc]

I am trying to learn how NX works and how I can do some things that sometimes I do with Solidedge and that sometimes help me to repair a mistake or save time.
In this case, I was trying to check what happened if I had to repair a link of a part that I have already renamed (I know I can rename it back, open NX and then do "save-as", change a link in several drawings or make several similar drawings of very similar models by copying and renaming the part and then copying and changing links in the drawings files (Not the ususal way of doing thinks but sometimes useful). That is why I wanted to rename parts in windows, in order to put NX in the worst situaion I could think of, and I am glad that NX can solve the problem just in case it is needed. Anyway, I take your advise and I will try to do things by " save-as" whenever it is posible.

Sorry about my English, maybe sometimes I don't explain myself in a proper way.

 

[cowski]

Yes, most links can be repaired in NX. If the file makes heavy use of wave linked geometry, repairing the links can cause a big headache. Beware of files that use the "promote body" function, as you cannot re-link broken promote body features.

www.nxjournaling.com

 

[Javiduc]

Thanks for the warning. That is a problem, because if I need to make a feature like multiple holes in an assembly I only know a way to do it that is promoting bodies. Is there a better way of doing that? By the way, I don't understand why in NX It is needed to promote body in order to make holes to multiples parts while in order softwares like SolidEdge it isn't needed.
If I use promote body and later I need to rename one of the part promoted, then I have to rename the part in assembly enviroment. Am I right?

 

[NutAce]

No need to use promoted body...
If you want to create holes for bolts (or the like), you can use the Hole Series from the Hole Feature. This will create a hole running through the selected components of an assembly...
Another option would be to use the assembly cut which does basically the same but you need to create an extrusion first which you then subtract from your assembly.

Ronald van den Broek
Senior Application Engineer
Winterthur Gas & Diesel Ltd
NX9 / TC10.1.2
HPZ420 Intel(R) Xeon(R) CPU E5-1620 0 @ 3.60GHz, 32 Gb Win7 64B
Nvidea Quadro4000 2048MB DDR5

HP Zbook15
Intel(R) Core(TM) i7-4800MQ
CPU @ 2.70 GHz Win7 64b
Nvidia K1100M 2048 MB DDR5