Control what happens after you Close a single part file

[keith2034]

thread561-203134
I read on line that starting in NX 5 you can set a Customer Default that will control what happens after you Close a single part file.

I want to close the part file window but now close the part in the assembly I am working on that uses the part.

Can someone tell me how to change this default value?

Thanks, Keith

 

[phillpd]

Customer Defaults->General->Part ... scroll to the bottom, i think that's the option you're referring to.

NX 9.0.3.4
NX 11.0.0.33 (Testing)
Windows 7 (Windows 8.1 Tablet)

 

[Toost]

I am not sure we speak about the same thing here.
You want to close the window for the detail file but it should stay open in the Assembly file ?

If so, this is a misconception on how NX works.
When you open an assembly , NX will load all files which are part of that assembly, including the "detail" mentioned above.
per default NX uses "partial loading" which means it reads as little as possible to show the detail in the assembly.
note that NX never copies the geometry from the detail into the assembly. The geometry from the detail file is shown in the assembly, if that detail file is missing when loading , the detail will not be shown in the assembly.
when you make some detail the work part or displayed part, the remaining of that file will be read from disk and that file will be "fully loaded" in the session. This state will make the name of that file appear under the "window".

If you close that file, you will also close the file from the assembly because there is only one set of geometry , and that "lives" in the detail file.
There is no way of making a file go from fully loaded to partially loaded.

Ok ?

Regards,
Tomas

 

[cowski]

When I want to remove a part from the "window" list, but keep it in the assembly, I close the part (right click on the part in the ANT -> close -> part); this closes it completely as outlined by Toost above. Then I click the checkbox next to the component, this reloads the component into the assembly, but the part file does not show up in the "window" list (at least not until I make it the work or displayed part).

I've heard that there have been improvements in the interface to switch between parts in NX 11. I've not had a chance to try it yet, but hopefully it will make life easier.

www.nxjournaling.com

 

[keith2034]

The cowski work flow is an improvement over what I was doing.

Thanks for the responses.

Keith

 

[Toost]

I don't really understand why one would like to get rid of the file name from the "window pulldown", ?
I have a colleague whose background was Inventor, and he was very eager to get the file name off the window pulldown.
I still don't understand why.
So, the file is open, and ?

Regards,
Tomas

 

[Javiduc]

I came from Solidedge and for me is strange to have so many "Windows" opened with different parts, a bit confusing when doing ctrl+tab and I sometimes have problems with some workflows, for example when I open a drafting (master model approach) then set the geometry part as displayed part, when I have finished modifing part I am used to go back not changing windows but closing the geometry window and in NX I have to "reopen" the geometry part in the drawing navigator.

I think a way of not closing part if you close windows would be good, but it is not an important issue I prefer NX development effords to go to most important things because I think I can get used to have a lot of windows opened and not close them after finising editing.

 

[Toost]

I almost never use the Window pull down.
Instead I use the Assembly navigator,:
When you look at the drawing, RMB on the model- Make Displayed part.
When you look at the model ( and the drawing file or Assembly above is open in the session) Display Parent - "select parent".


Regards,
Tomas