[NX 8] Drafting question (tracelines and lightweight) 1

[cubalibre000]

Hi,
It's possible change a full loaded assembly base view in a lightweight base view and vice-versa ?
It's possible disable tracelines in a view ?

Thank you...

Using NX 8 and TC8.3

 

[JohnRBaker]

There is no such thing a 'lightweight' view in Drafting. The closest we have at the moment is to select the Drawing view(s) of interest, press MB3 and select the 'Style' option. Now open the 'General' tab and near the bottom of the dialog change the 'Extracted Edges' option from 'None' to 'Associative'. Then hit OK. Now you can open the Drawing, add additional notes and dimensions as well as generate plots or PDF's, all without having to open any of the Components in the Master Model Drawing. This will reduce the memory needed to open the assembly, effectively making it 'lightweight'. Anyway, that's the best that we have for now.

As for 'tracelines', I'm not exactly sure what it that you're talking about. Could you be more clear and perhaps provide a picture of what it is that you're concerned about.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

UG/NX Museum:

http://www.plmworld.org/p/cm/ld/fid=209

To an Engineer, the glass is twice as big as it needs to be.

 

[cubalibre000]

John,
Lightweight representations are faceted versions of the solid bodies and sheet bodies of a component. Faceted bodies are often used as alternative representations of the components and can improve performance, especially in large assemblies.
This come from CAST Online Library.
So when I add base view, I can us this option to improver performance (as image attached).
Can I switch from faceted to no and viceversa ?
Can I switch from tracelines enabled to no and viceversa ?(as image attached).
Can I switch from an exploded view to no and viceversa ?


Thank you...

Using NX 8 and TC8.3

 

[JohnRBaker]

OK, while it is true that you can place a Faceted (i.e. Lightweight) hidden-line view(s) on a Drawing, I think you will soon notice that they do not provide the 'quality' of either the HLR or the rendering of the edges that most people expect in a Drawing. What I mean is that once this sort of view is placed, it's appearance cannot be edited (improved) so 'what-you-see-is-what-you-get', and this includes when you plot it or export it to a .pdf file.

If you follow my original recommendation to use the Extracted Edges option, once all your views are created (and their edges extracted), when you open your Drawing in the future without loading any of the Components (per Load Option settings), this will also result in using as little memory as possible. And the added advantage is the 'quality' of the rendering, Hidden-Line as well as the normal model edges, will be more than suitable for recreating high-quality plots and .pdf files.

As for the 'Tracelines' I think you will just need to go back to the Exploded View(s) and simple NOT create the Tracelines to start with (and if they already exist, delete them).

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

UG/NX Museum:

http://www.plmworld.org/p/cm/ld/fid=209

To an Engineer, the glass is twice as big as it needs to be.

 

[RAMNX]

Regarding tracelines we can use view dependent edit and make the lines invisible also

 

[vriyg]

NX8 doesn't support (or rather create) "ligthweight faceted Reference sets", how has it been replaced? We used that extensively... Thanks.

 

[JohnRBaker]

Actually the changes were made in NX 7.5. Lightweight Representations are now part of the model itself and no longer depends on the use of Reference Sets. Rather they are simply enabled by a setting on the Load Options dialog. Also you can explicitly change a Component from Lightweight to Exact or vice versa from the Assembly Navigator. That being said, it's best to just leave your system settings to their out-of-the-box values and let the system take care of things for you. One recommendation, particularly if you use any Family Table or reuse library parts, is to do a complete refile of ALL of your parts before continuing so as to get maximum value from the Lightweight change that were made in NX 7.5.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

UG/NX Museum:

http://www.plmworld.org/p/cm/ld/fid=209

To an Engineer, the glass is twice as big as it needs to be.