Hidden lines NX10 5

[ElconCAD]

thread561-295526

Does anyone know if the method described by TOOST still valid in NX10. I have not had any luck after upgrading from NX8.5.

The method involves using view dependent edit to show individually selected lines as hidden.

 

[Arkance/PhoeNX]

I just tried the same part in NX8.5 and NX10 and the method doesn't work in NX10 that I can see.

Anthony Galante
Senior Support Engineer


NX3 to NX10 with almost every MR (21versions)

 

[ElconCAD]

Very odd that such a useful tool be removed. Is there a alternative solution available?

 

[Toost]

oops, this is a regression.
I spoke to Gtac.
IR8281308


It seems that the new exact views does not have this option where manual edits has precedence over system edits.
the view type "Exact (pre NX8.5)" still has this function.
the "exact (pre NX8.5)" view type can be enabled under Customer defaults. ( it then becomes available in the settings.)
It seems that this change was implemented in NX8.5. We still run NX7.5 in production why i have not seen this before.

Regards,
Tomas

 

[cowski]

I'm wondering what advantage the new "exact" view provides. This is the second instance I've seen where it provides less functionality/usability than the "exact (pre-NX8.5)" view type.

Edit: I went back to the NX 8.5 help files to get more info on the "exact" view type. It seems the main advantage is that you can view and annotate existing views without loading the component geometry. It looks to have the same functionality as the "pre-NX 8.5 exact view with extracted edges". So, perhaps the question becomes, "Does the view dependent edit workflow described in the other thread work in a "pre-NX 8.5 exact view with extracted edges"? If it works there, then it would seem that the new "exact" view type is really a regression.

www.nxjournaling.com

 

[Toost]

It will be interesting to see if this function has been deliberately removed from the newer view type or not.
One of the current catchphrases is "discoverability", and the "reverse order edit" is a bit difficult to discover by oneself.
The method is still most often way more effective/faster than erasing the stuff that shouldn't be visible in the view.

Regards,
Tomas

 

[ElconCAD]

Agree with the above statements. It was a of tremendous benefit learning that method when I first came across it on this forum. Saved our company a enormous amount of work hours. Now that's gone and I have to explain to my supervisors why It takes longer to clean up a drawing, because its back to the tedious task of single eliminating 990 lines display 10. There skeptical at the moment, But seriously "upgrading" should mean more not less!

 

[Toost]

I got response from GTAC .
It turns out that this is now a documented process in NX ( Which i think that the "old process" wasn't)
The difference is that one has to KEEP the hidden lines setting = DASHED( RMB- View- Style)
AND turn on "Show Referenced Edges Only". ( Same dialog.)

The new procedure :

1) place the view , set all hidden edges set to Dotted.
( and maybe the color that you want the dashed edges to have)
2) Do the View dependent edit , edit the edges to Dashed font.
( now you can see the difference between the manually edited and the non-edited in the dotted /dashed.)
3)RMB the view - Settings - hidden lines : turn on "Show referenced Edges Only"
The manually edited stays dashed whilst all other disappears.

Do NOT set the hidden edges = invisible after the above, it will erase the view dependent edit....

I am not sure that this is a better process than the old. But it is covered in the manual.

Regards,
Tomas