Optimized setting for large assembly drawing VIew.

[ninjaz]

Which one of this setting will consume less memory . Style --> Extracted edges-->None or Style-->extracted edges-->Non- associative.

Note:The drawing view is just for illustration purpose .which consists of huge CAD parts. DImensioning is not necessary in the views.

 

[JohnRBaker]

Well the extracted edges, associative or otherwise (if you do nothing else but set the extraction option), will make the file size larger, which means that it will require a bit more memory to open the Drawing. Now since you've set the extracted edge view non-associative, if the drawing changes there will be no additional overheard (i.e. memory) needed when the Drawing is updated since the drawing will not update (being non-associative).

That being said, the primary reason for even extracting edges, particularly if you leave them associative, is that the NEXT time you open the Master Model Drawing, you don't have to open any of the 'assembly' Components, which will significantly reduce the memory, and thus the time needed to open the Drawing. You can continue to open the Drawing, add dimensions, annotations, notes and labels, fill in tables, etc. all without having to open any of the Components. And when changes are made to any of the Components or you need to add an additional view, like a Detail view or a Section view, all you need to do is fully open the Master Model Drawing once, update all the views, make your changes (if you're actually adding additional views, be sure to extract the edges of these views as well) and save the Drawing file and then you can go back to working on the Drawing without its Components until it's time to update for changes in the detailed models. This can significantly help to improve performance (when opening only the Drawing but none of the Components) when working with Drawings of large complex products.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[ninjaz]

Thanks John. I understand the explanation. Your explanation mainly deals with updating the drawing.

But i have issues for even creating the base views for first time itself. Some times i will get out of memory error. So, if i want to get rid of the out of memory error . i must set an optimized view parameters.

Is it possible to comment in this perspective( for creating a large assy view for first time).?

UG-7.5 , windows XP.

 

[JohnRBaker]

Are you running 32-bit or 64-bit version of NX? If you're not running 64-bit, then you need to move there ASAP.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[EnJoeNeer]

Be sure to verify that "Use Lightweight Representations" is checked in your load options. That is commonly the difference between a good and bad day, but as John says, if you're not in 64bit, get there.

 

[EnJoeNeer]

....I should mention, drawings always load exact representations for visual purposes. But, depending on what else you have running and what operating system you're using, it can still help you out.

 

[SDETERS]

Could you also turn on simplify small feature under view style under the hidden line tabs? Would this help at all?

 

[JohnRBaker]

One thing that you should do is go to...

Customer Defaults -> Drafting -> View -> Threads

...and make sure the 'True Hidden Line' option is toggled OFF.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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