Changing a View Type. 1

The choice is made at the time when you add the views and can't be changed thereafter. It is grayed out. If you were able to do that then you would still lose the associativity of whatever dimensions you had previously added because the rendered elements are different.

Best Regards

Hudson

When creating views of large assemblies, try using the assembly hidden line function (view > visualisation > assembly hidden line) you need to orient each view of the model one at a time and save the view from within the command. You can then add the new created wire frame out put into the drafting (model view though)on different layers and then on the drafting sheet add your views and make the right layer containing your curves visible in view for each view. You will then have an exceptionally lightweight drawing to which you can dimension etc without all the hassle of massive updates.

Hope this helps

Simon

Simon,

We used to use that but I believe the later added view based on facets functionality to be superior and far easier to manage. What the (view > visualization > assembly hidden line), method does is to output curves usually large numbers for large assemblies, which you can then save to a file and add into your drawing in lieu of models on the face of the drawing. The newer functionality will allow you to maintain those views far more easily as the models change, and it is lighter weight to manage than solid models.

To give you an example I tried it with NX-4 using a reasonable sized assembly and it is very fast indeed, both to create and to update views. Dimensions for features including centerlines and radii also appear to apply normally. I don't do too much drawing these days, but this functionality seems pretty good to me .

Best Regards

Hudson

Hudson

Interesting, I've not seen that before, so let me get this straight so I can inform my users. If we are working with a large assembly and wish to create light weight views which will not take an eternity to update, we can, when we first add a view choose to make it faceted representation only? But once the view is added, then we cannot change it? click this link to see if I'm singing from the same hymn sheet as you.



Many thanks

Simon

Also note that in addition to adding dimensions to faceted views, that you can also create section views from a faceted view. Granted, the section view will NOT be faceted, but using this work-flow will still help to keep your drawing update times and performance optimal.

The biggest downside when using faceted views on a drawing is that once created you can't change the tolerance used to create the view unless you have an 'Advanced Assembly' license (to access the facet generation functions directly where you can then edit the tolerance used to define the existing faceted models in drawing). Now this is generally not been a problem since the customers who are creating assemblies so large that there are drafting issues, have generally already purchased 'Advanced Assemblies' licenses for the other benefits that it offers customers with large and complex products.

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

Simon,

Normally I'm a tone deaf atheist, but yes we're doing it the same way. I haven'y used this much myself but as I said I put it through its paces recently after I realized that I had neglected it and was pretty impressed with the result.

Gotta love that Jing

John explained anything else you needed to know

Regards

Hudson

John

Excuse my ignorance here, we do have advanced assemblies licences, but please can you clarify where I go to change the tolerances of facets if I need to.

Many thanks

Simon.

Hmmm.

I've just tried it on a large assembly and it still eats up the performance to a point where the machine is just ticking over. I've attached a JPEG to this post of the assembly I was working on. Perhaps I'm missinga trick

regards

Simon.

Open the assembly as facets or reps to save memory and the drafting will still work.

No you didn't attach a Jpeg!

Regards

Hudson

Simon,

OK, to update the apparent tolerance of the faceted bodies used in the drawing, which effects such things as the quality of plots, while in the drawing part file, but in the modeling module, go to Assemblies -> Advanced -> Representations... Once the 'Define Representations' dialog is displayed select the 'Edit Facet Parameters' button. When this dialog opens, select the 'Select All' button and hit OK and in the next dialog, adjust the 'Distance Tolerance' to the desired level.

As for the issue of memory usage when working in a large drawing if you first use faceted views for all normal views and if after creating any section or other views, any that are not using facets, go to Edit -> View and select those non-facet views and turn the 'Extracted Edges' ON and then save your drawing file (this can all be done before you actually state adding dimensions and other annotation such as notes and labels. Once this had been done, you can now open the Drawing file WITHOUT having to load ANY components (however you must set your Preferences -> Drafting -> View update option to 'Delay View Update'). This will provide the maximum benefit in terms of freeing up memory and improving system performance when you need to open the drawing in the future, either to add or edit dimensions and annotations, or when you need to generate documents such as paper plots or PDF documents.

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

Hudson

Sorry, jpg now attached.

Simon

Simon,

You'll also want to turn off the shaded display during view placement.

I tried opening as reps more of a vehicle design than good judgment would recommend. All the floor pan sheet metal panels interior including, seats carpets, IP and console, pedals carpets, door trims and garnishes. Then I open a vehicle exterior with all panels sans underbody. Either of these seem to be at the limit for the number of parts that the computer will allow me to open. In both cases it took about a minute to generate the views. I would not using solid bodies attempt to create these views. Ever! Half that geometry would certainly be too much for the system to handle.

Best Regards

Hudson

We have in the past opened the master assembly as facet reps adn used these for the drawing, the problem is that (as far as I'm aware) that facets are completely useless for anything other than visualisation, you can't accurately dimension so them which is ultimately what we want to do for our homologation drawings, unless you change the setting when adding the view as discussed by John earlier in the thread, however to use those, you need the model to be fully open as if you open the model with reps, then the views you add to the drawing are useless other than for visualisation.

Regards

Simon.

Well, it gives you a distance and a radius. fairly reliably, I have only tested it a bit and passed it on to a few drafters for the machine layout drawings. As I said it certainly makes the difference between fast and impossible for really huge assemblies. I wouldn't use it for component drawings, as we would seldom consider it necessary to do so.

Have you examples where it differs dramatically from the solid to the faceted view whereby the size of the returned dimension differs critically?

I'm interested to hear whether the balloon ID for a pasts list will work in that regard, and to confirm that hide component in view performs reliably.

best regards

Hudson