Update View takes too long 6

[BOPdesigner]

Are there any tricks to getting drawing views to update faster in NX 6? I have always noticed that other CAD systems don't seem to struggle with this as NX does. Have a view that takes 5 minutes to update. Another user has one that takes much longer, probably over an hour but don't know for sure because he always kills the application because he can't wait any longer.

 

[JohnRBaker]

It's the computation of the hidden-lines that generally causes the long updates. There are several things that you can do in NX to limit the impact of these view updates. One thing is to make sure that in your Drafting Preferences that you've toggled the View Update option 'Delay View Updates' to ON and perhaps you may even wish to toggled ON the other option, 'Delay Update on Creation', as well.

While neither of these will have any impact on how long it takes to update Drawing views, they will allow you to control exactly when the update does place so that you don't have to wait every time some minor change is made. You can delay the actual update until later (you could even write a simple NX Open program which could be used to update drawings offline).

Also, if you get to a state where you would to delay 100% the updating any anything on a Drawing you can also Extract Edges in each Drawing view and then NOT load the master model and the drawing will remain unchanged from the last time it was updated.

Note that this is one of the areas where multi-core CPU's could offer at least some help since Hidden-Line generation is one of the limited number of areas in NX which is multi-threaded.

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

http://www.siemens.com/plm

http://www.plmworld.org/museum/

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

 

[BOPdesigner]

Thanks I am aware of these settings. It is purely in the computation time where my concern lies. Wondering what NX is doing different from what other CAD systems are that makes it so much slower.

 

[JohnRBaker]

Giving you the CORRECT hidden line views?

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

http://www.siemens.com/plm

http://www.plmworld.org/museum/

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

 

[BOPdesigner]

Yes, hidden lines set to invisible. When I get a chance I will do a comparison of the same model in Solidworks and maybe Inventor.

 

[UGoverALL]

Very often long computation time on View Update is linked to the fact that the assembly is not very good as quality.
Suggestions:
1) Refile all your part to the correct NX version
2) Part Cleanup on every 3D parts (or at least on the assembly and drawing files).
3) Verify that none of your parts have "consistency" problems (hope you've a Checkmate tool that automatically verify it).



Beppe Grimaldi
SISW Italy

 

[JohnRBaker]

I JUST remembered one other thing that you need to check.

Go to...

Customer Defaults -> Drafting -> View -> Threads

...and toggled OFF the option titled 'True Hidden Line'.

Now don't be too worried that somehow this will cause the hidden line views to be rendered incorrectly or cause them to look weird. This option ONLY effects how symbolic threads are rendered in hidden-line views. For the vast majority of people, turning this OFF will never be noticed in terms of the quality of their plotted images (with a few exceptions, which is why the option is there in the first place, but the conditions where this would be true are very rare and very part and workflow specific), but it COULD improve display performance when updating Drawing Views. However, there is no guarantee, but under the right conditions...

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

http://www.siemens.com/plm

http://www.plmworld.org/museum/

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

 

[BOPdesigner]

That is already turned off. So here is the deal: Assembly has components from NX 4 thru NX 6. I ran the part clean up on everything and saved them in NX 6. That improved update time by about 30 seconds, from 17 minutes 20 seconds to 16 minutes 50 seconds (so not much of an improvement). This is with 64 bit NX 6.

Next, I STEPed the assembly out and recreated a similar view in Solidworks which takes 1 minute and 50 seconds to update. To compare apples to apples I imported the STEP assembly back into NX 6 and created a similar view and it takes only 1 minute and 20 seconds to update. These STEP based views are on 32 bit NX on a different machine.

So... Can somebody explain what the heck NX is doing in the background during the drawing update such that it takes 17 minutes to update the view with the native data? Is it evaluating assembly constraints? WAVE links? etc. If I have unresolved constraints/WAVE links would that affect it? (please say no) What can I try next? I can't even update the view with the native CAD data on the 32 bit machine.

 

[doc1955]

I've had the same problem we are using NX5 installed on a 64 bit platform with 8 gig of ram. Some drawing you change anything on the drawing you may as well go out for some donuts and coffee. I ran across some assemblies that in modeling it will do the same just sit there and update for about (a couple files) fifteen minuts. I did send one into GTAC but it never did get resolved and I gave up!

Doc

http://www.goodrich.com

 

[chuckrow]

We have had the same problem along with one concerning the new constraining methods. It has been our unfortunate dilemma to have a assy completely constrained only to have it blow apart the next day. I for one am a bit disconcerted over the uniqueness that was UG being usurped by the latest versions into a system that seems to be "copying" others..ie solid works for one..this is a marketing strategy that allows a source to discontinue support for a older version by constantly "improving" the software..thus forcing us to buy the new. The time involved with updating views is just typical of a system that truly tries to do too much for the user..I understand about the settings and although many companies are leaving the ability to adjust customer settings the lengthy waits are unjustified. All of this comes as most companies require a BA for a NX user..they want to consolidate engineers with NX 'users'. One prob ive had is that most my degreed 'users' i wouldnt recognize unless i see their rings while they are picking their noses.

 

[chuckrow]

That is already turned off. So here is the deal: Assembly has components from NX 4 thru NX 6. I ran the part clean up on everything and saved them in NX 6. That improved update time by about 30 seconds, from 17 minutes 20 seconds to 16 minutes 50 seconds (so not much of an improvement). This is with 64 bit NX 6.



Next, I STEPed the assembly out and recreated a similar view in Solidworks which takes 1 minute and 50 seconds to update. To compare apples to apples I imported the STEP assembly back into NX 6 and created a similar view and it takes only 1 minute and 20 seconds to update. These STEP based views are on 32 bit NX on a different machine.

So... Can somebody explain what the heck NX is doing in the background during the drawing update such that it takes 17 minutes to update the view with the native data? Is it evaluating assembly constraints? WAVE links? etc. If I have unresolved constraints/WAVE links would that affect it? (please say no) What can I try next? I can't even update the view with the native CAD data on the 32 bit machine.


This is a typical problem..we have offshore workers ie.india that dont want to conform to our standards and continually use wave geometry and also use routing operators for simple hoses..adds a huge weight to the file. The software apparently thinks it has to update every link, file, line, spline.. etc etc in the asm EVEN though none of said were involved in the change..i have heard the expression that while waiting for a update on NX a wheel fell off a car out in prototype build area..thus due to a update to something totaly uninvolved..

 

[thom9446]

BOPdesigner: I have been complaining recently about these issues as well. John, it's interesting that you say that you say hidden lines is hyper-thread supported because my system (a hyper threaded Xeon-Quad core) tops out at around 15% CPU usage and it still takes a really long time to update.

I recently did a similar test where I created a parasolid of a large assembly and imported that back into NX and SolidWorks. SolidWorks used about 60% of the CPU power and did the view updates about 65% faster than NX did. What gives? We have a lot of down town around here waiting for drawings to update (and yes, we have done all of the previous suggestions the help reduce this).

chuckrow: We have had similar issues with constraints and have been in contact with GTAC about them. We save a large assembly that is fully constrained with no errors, and the next day we open it, only to find some constraints are broken while others have completely disappererd. Very fruststrating.

 

[BOPdesigner]

Issue has surfaced again with a different assembly this time. As I am typing this only one of my 4 cores is doing any work. Why can't all of them be working on the task? Headed to lunch. Hopefully the view is placed when I get back.

 

[capnhook]

There's a bit of background on this problem in this recent thread:

http://www.eng-tips.com/viewthread.cfm?qid=281143

..

Proud Member of the Reality-Based Community..

 

[BOPdesigner]

Thanks capnhook. Pretty much the same issue. It actually took between 7 and 8 hours to place the view (with updated after placement turned on). Assembly has 160 components. Data size on disk about 300 MB. I would call 2/3 of the components heavy. So today I am experimenting. I placed the view with hidden lines turned off and no update after placement. That worked ok (within about 5 minutes). Then I went and put a bunch of the components that are not shown within the view in a different layer in modeling. Then made that layer invisible in the drawing view. Is this the recommended approach? Now I turned hidden lines on and that thread rendering turned off and I am updating the view. Still it is taking too long....

 

[BOPdesigner]

This issue has cropped up again with a certain assembly. And so I wanted to get your feedback on what criteria is used to guage the size of an assembly. How do you define a large assembly? By number of components? By complexity of geometry? For example I have one assembly in another CAD program that has 365 components, and 12,800 faces. The current NX model that is giving us problems has a subassembly which has only 27 components, but 23,800 faces. Which takes the biggest toll on model manipulation (rotate, pan, etc.) and drawing view creation/update time? To continue, there are several instances of this NX subassembly in a top level assembly combined with other components of complex geometry which results in a model which has 1000 components and over 533,000 faces. Is this considered large? I am looking at some of the different techniques like simple reference sets, extracted bodies, simplify assembly, suppression by assembly arrangement etc. to see the impact. Here is what I have found so far. It took 30+ hours to place a standard drawing view of the assembly. Then I created an assembly arrangement which suppresses all the internal components resulting in a reduction from 1000 -> 149 components and 533,000 -> 32,000 faces. Good news is that now the drawing view placement only takes one minute or less, this is an acceptable wait time for the view placement. However the unanswered question that exists is this. Why is it I can open the same assembly in another CAD system and place an associative drawing view in that same one minute or less without going through the time and effort to suppress the internal components? Sorry for all the rambling, just trying to get to the root(s) of the issues here. Also, many of the complex geometry parts are imported vendor parts (STEP, IGES) and they contain some errors when you run the Examine Geometry operation. Would this have any impact on drawing view creation time?

 

[capnhook]

Nearly a year has gone by since this thread was started. Looks like we are all still affected by this problem.

Does anyone know anyone at GTAC that feels our pain? My experience is that big issues like this just don't ever get resolved, we get tired of looking for help, and nothing gets done. The root of this problem is not being identified or addressed or fixed.

All I hear is the ocean.......when I put my mouse to my ear. I was hoping for more.

Thanks for your work on this, BOPdesigner.

Proud Member of the Reality-Based Community..

 

[daluigi]

We've this 'update' issue since our move to NX6.
When NX4 was very fast on everything, NX6 now goes into update workflows after a lot of actions and the new assembly constraints patterns certainly makes it more terrible.
A lot of complains already in the GTAC database but always the same old same 'will be resolve by code change blabla' when there's simply an answer...
NX6 is really the worst of all UG versions.

We can't ear the ocean here but the infinite silent space.

 

[JohnRBaker]

If you honestly think that NX 6.0 "is really the worst of all UG versions" than why are you NOT running NX 7.5? After all, it has been available for OVER A YEAR!

The changes which we have been making, and continue to make, to improve performance will only be of benefit to you if and when you upgrade to the most recent releases.

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

http://www.siemens.com/plm

http://www.plmworld.org/museum/

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

 

[capnhook]

7.5.x.x drawing view updating is what I have posted about. Never used NX4 through NX6. Used just about everything NX3 and previous.

I am a 7.5.x.x user now, and am experiencing the same problems with view updating as these other users are experiencing, and have for about a year, now.

All I hear is the ocean.........


Proud Member of the Reality-Based Community..