Update Display options?

[JMagnus]

Is there any way to get NX10 to periodically update display automatically? Like set it on a timer to do it every 10 seconds or so?

I do a lot of gaming at home and I know that the two drivers for each type of graphics are COMPLETELY different, but I feel like it should be able to globally update display constantly as you rotate/zoom etc.

Thanks in advance!

 

[Xwheelguy]

Nope, not that I am aware.

You can set your facets to a higher resolution/detail as well as updating every facet, not just what is shown onscreen. Doing so will impact graphics performance negatively, depending upon your hardware, etc.

Tim Flater
NX Designer
NX 9.0.3.4 Win7 Pro x64 SP1
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB

 

[JMagnus]

Yeah, I did set all my stuff up so that it works best for me. Kinda have a beast PC here. Quadro K2000 32GB RAM Intel Xeon E5-1620. So, the thing should be able to handle it, I just think there should be an option. Mostly due to the fact that each time I hit "Update Display" it instantly fixes everything with no issues. But, cranking up the detail doesn't keep it from displaying the broken circles for some reason?

 

[cowski]

Check out thread561-379803
robnewcomb provides a link to a document that describes the options that control display tessellation.

edit: forgot to mention that the document pertains to the tessellation of individual part files. If you are working in an assembly with "lightweight" representations of the components, the settings discussed in the document probably won't help you.

www.nxjournaling.com

 

[JohnRBaker]

Why exactly do you feel that you need something like this? What 'problem' do you think that something like this would solve? Please provide an image or video clip if that's what it takes to show us what you think the issue is.

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

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

 

[JMagnus]

John,

It's not so much a "problem" as it is a "nuisance". I make a single component my work part, adjust something like hole distance, then save the part. Then I display parent, go back to my main assembly and everywhere that component is, half the holes have diamond shaped holes that make it a little more difficult to pick the centerline to constrain it into position. I'm trying the part/view/fixed faceting scale thing right now as we speak.

I'm not really allowed to post up images, per my company's orders.

Reason for edit: changing from "part" to "view" has fixed the "nuisance" so far. Thanks for the link to the document about tessellation lines and facets

 

[JohnRBaker]

One thing that you could do is NOT open your Assemblies using Lightweight Representations (this is a setting in Load Options). Now if you're dealing with large complex Assemblies this will not be as efficient but it will mitigate the change in appearance of a Component when it's the Work Part verse when the Assembly is the Work Part.

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

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

 

[JMagnus]

I shut off the lightweight and partial loading every single day Our admins have them set so that I can't even change the defaults to shut them off permanently. I do work in extremely large complex assemblies with over 4000 parts in them, but it seems like with NX10, everything has been significantly improved. Performance is outstanding in NX10! just wanted to figure out how to get it to update the holes. Thanks again for your help! If you can, can you answer my other thread about solidworks files from NX please? Since you are the guru and all #worshipjohnbaker

 

[JohnRBaker]

Don't shut off the 'Partial Loading' as that has no effect whatsoever on model display.

I assume that you're working in the Shaded mode and not 'Static Wireframe', correct? If you're already not using Lightweight Representations, have you looked at the new Visualization Preferences for Faceting? In the Part Settings/Shaded Views section of the dialog, try setting the Facet Scale to 'Fixed' and then pick a desired resolution. BTW, don't toggle ON the 'Align Facets along Edges' option as that will just slow things down and it's only really needed if you're creating high quality images on the screen.

But please note that irrespective of how a 'hole' might appear, it will still behave like any other hole in terms of selecting and referencing its edges. Unless you're running in the 'Static Wireframe' display mode, you're always going to be getting some level of 'faceting' of edges. That's just the way any realtime shaded display is going to work.

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

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

 

[cowski]

I'd recommend that you keep partial loading turned on. It has nothing to do with your display issues but it can reduce the memory usage when working with an assembly.

www.nxjournaling.com

 

[JMagnus]

Guys,

I turn off partial loading because frequently I'm working on individual pieces updating them in the context of their large assembly. Once upon a time, I tried updating something and NX gave me an error saying "part is not fully loaded and the operation has failed" or something along those lines. If you guys can tell me that particular situation was just a fluke, and the partial loading has ZERO effect on things like JT previous, dataset management, added operations or features to parts, any post part data such as product views. I don't turn it off for the sake of visual performance. It just seems that my exploded views, PMI, model views, and assembly management seems to maintain a lot better since I have been using a fully loaded component.

As previously mentioned, I have 32 gigs of RAM so memory really shouldn't be an issue. I have only seen my session as high as 27 gigs and that was because I was loading about 16000 pieces into one session.

I'm using the Visualization preferences, and the option just below it "Visualization Performance". I like the new options to be able to change that stuff. My graphics card struggled to keep up in NX9 without any options modified. (I know NX9 had modifiable options, I just never noticed them until NX10) My parts now all look a little cartoon-like but it rotates a lot smoother. I run in "Studio" mode 100% of the time. Should I use "Shaded with Edges" instead? It seems to make no difference in performance.

Also, thanks for the tip on 'Align Facets along Edges' luckily, I didn't have that toggled ON, and still don't.

Thanks for all the help again!

 

[JohnRBaker]

Unless you really want to see your model in some sort of 'aesthetic' presentation mode, I would not normally work in 'Studio' mode but if you say it has no impact on performance, well that's your call.

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

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

 

[JMagnus]

Any comments on the partial loading thing?

 

[cowski]

I always use partial loading and I can't recall ever having an issue like what you described. The way partial loading is supposed to work is that only the geometry needed for representation in the assembly is loaded; if/when you make a part the work part, NX will fully load that part. It is generally a pretty seamless operation, unless you are working with a particularly complex part in which case it may take a few moments to load fully.

www.nxjournaling.com

 

[SDETERS]

I have had a couple issues in NX8.5 and teamcenter using partial loading. I keep it turned on until I get an error saying my assembly will not open. Once I get this error (I can not remember what it says at the current time 'Something about not having shape") I turn partial loading off and the assembly loads just fine. Which in turn I have to save the assembly, which in turn saves all the parts in the session that NX has read write access to. Which puts a last modify marker by me on parts I did not even modify. Turning this setting off is my first go to try when an assembly does not open. For what it is worth.

 

[cowski]

SDETERS,
When you save the assembly, make it the work part then use "save work part only"; that way it will not attempt to save all the components.

www.nxjournaling.com

 

[JMagnus]

but cowski, what if you worked a few of those parts and not all of them?? I hit the basic "Save" that says "Saves the work part and any modifiedcomponents". For my experience, any time you pretty much load anything and rotate the screen, it considers you "modifying" it and tries to save a bunch of stuff you didn't actually work on.

 

[JohnRBaker]

Making a Component Part the Work Part, or even the Displayed Part, and if you even "rotate the screen", this will NOT mark the Component as 'modified'. However, many times component parts may not have been updated to the latest version of NX and therefore the simple act of opening a part will mark it as 'modified'. But even if that is the case, the suggestion that cowski made is still a valid workflow, simply use the 'Save Work Part Only' option and this will ONLY save the main Assembly and NONE of the Components, whether they've been marked as 'modified' or not.

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

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

 

[JMagnus]

well I guess I could just start saving "work part only" each time I adjust something on a single part. That makes sense, I will do that from now on... Thanks guys!

^^not being sarcastic, being sincere

 

[NutAce]

I shut off the lightweight and partial loading every single day Our admins have them set so that I can't even change the defaults to shut them off permanently.

You should always be able to save your load options as a User setting.
In the assembly load options at the bottom in the Saved Load Options section you can select "Save as Default". This is on user level.

Ronald van den Broek
Senior Application Engineer
Winterthur Gas & Diesel Ltd
NX8.5.3 / TC9.1.2
HPZ420 Intel(R) Xeon(R) CPU E5-1620 0 @ 3.60GHz, 32 Gb Win7 64B
Nvidea Quadro4000 2048MB DDR5

HP Zbook15
Intel(R) Core(TM) i7-4800MQ
CPU @ 2.70 GHz Win7 64b
Nvidia K1100M 2048 MB DDR5