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]

Have you contacted GTAC and have they verified that you're running a reasonable configuration? Have you ever submitted any examples for GTAC and or development to look at? And when you say 'view' I assume that you're talking about views on a Drawing sheet, correct? If so, may I suggest that you check the following item:

Customer Defaults -> Drafting -> View -> Threads

If the 'True Hidden Line' option is toggled ON, please toggle it OFF.

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]

1. yes

2. yup, did a couple of app-shares to confirm. Could not share the parts. By what I read here and elsewhere, there are other parts that were submitted by other users, that are taking way too long to re-draw. Another user at this site complains also, I know it is a big ocean, but I am not alone with this problem.

3. yessir

4. Toggled OFF -- only reccommendation I ever got from GTAC. Did not help.


No progress on this issue for me.


Proud Member of the Reality-Based Community..

 

[thom9446]

We too have issues with updating drawings. I've voiced my concern that I feel like Siemens is focusing all of their time on PMI or on those who work exclusively in 2D drafting while ignoring those of us who make 2D drawings of 3D models.

HOWEVER, I did want to make sure everyone knew that the number one voted on topic for drafting during the CIP process was improving large assembly drawing performance. Siemens is now required to devote at least one man year (I think that's right) to addressing this problem. To me this is encouraging, but I'm not holding my breath. I could spend one man year writing a romance novel and it would still turn out like crap (this may be a bad analogy because they're probably all crap, but you get the idea).

There were an overwhelming number of votes for this item so hopefully they get the picture.

Mike Thompson
Mechanical Engineer

http://www.wagstaff.com

 

[JohnRBaker]

You may also wish to look at the default display 'Tolerance' used when creating a Drawing. This can be found at...

Preferences -> View -> General

...as well as at...

Customer Defaults -> Drafting -> View -> General

...where it's identified as 'Chord Height Tolerance'.

If this value is set to zero (0.00) the system will assign a tolerance based on the size of the view/drawing, however this might be much tighter than it needs to be. I would recommend that you set it to something like 0.01 (or even 0.1) and see if that helps any.

Note that changing the Perference or Customer Default will only effect the next views which are added to a drawing (note that no matter what this setting is, a 'Projected View' will inherit the tolerance of the base view). So if you have an existing drawing, you will need to select the views of interest, press MB1, select 'Style' and then in the General tab change the value of 'Tolerance'. Also note the tolerance used to DISPLAY your drawing on the screen is NOT what is used when the drawing is finally plotted, so it can be much larger, giving you better interactive display performance. Then when it comes time to Plot your drawing, you can supply a totally different 'Tolerance', something more appropriate for your final hardcopy.

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]

Mr. Baker, this is what you once told me in another thread (above):

You've already been given everything that there is to be known about the Choral Height Tolerance. Our recommendation is to leave the Customer Default value set to 0.0 as this will allow the system to try and do what we feel is 'optimal'. However, I suspect that there is NO setting which will be a 'magic bullet' for your situation. Without having someone look over your shoulder at what you're doing, I don't know what else that anyone can do for you.

Has your recommendation to the user community just changed? I have tried changing this value, and it has not had that effect.

Oh, and that guy looking over my shoulder, that's just the ocean.......

Proud Member of the Reality-Based Community..

 

[Toost]

A few tips on drawing view update performance.
I have investigated the issue quite thorough.
The tips below will speed up the performance somewhat but there is no revolution.
Make sure all options that isn't very required is off. for example, setting the color of the visible lines to a specific color is probably not needed if it is going to be plotted in B/W. ( default = Blue which is an override, set to "none") Same w the color of the hidden lines. etc etc.)
Setting the color / font / width on a couple of hundred thousand objects will need computing power, which in the end sums up.

Make sure that there is nothing interfering or duplicate since that condition requires more computing.
All "fancy" options needs extra computing = extra update time ( example interference curves.)
The View tolerance ( discussed in other thread) has in my perception no major influence on the computing time. Leave the customer default = 0.0 and if something looks wrong, zoom the view to be ~full screen, set it to 0 and OK the View Style. NX will again find a new value since 0 is impossible but very likely the error is gone. ( -yes, the scale is depending on the zoom factor too.)

Watch the Task manager if running 32bit Windows and note if the Ugraf process goes above 1Gb, ( i cannot state a specific number here.)as soon as the computer starts swapping we are talking long process time and /or unfinished updates. 64 Bit computers with "enough" RAM will finish the updating but not run much faster.

If possible, simplify what is about to become a view, black dots on the plotted drawing, doesn't add anything to the process.
( "This minute dot on this drawing showing an entire car is the injection nozzle, yes the dot is the entire nozzle , with threads, holes, engravings and such")
The Hidden line calculation will calculate all objects no matter the size, even those that are too small to become more than a dot on the plotted paper. ( the ability to zoom in on the resulting view and see the details can often fool the user to keep the miniature details.)
Simplifications using Reference Sets and Arrangements.

Imported geometry such as Step files quite often carry problems for the hidden line calculations. Run Examine geometry + manual cleaning + Part cleanup. As noted before, duplicate geometry is difficult to calculate / decide what surface should be visible and which not. Using the Section tool ( Clip work section in 7.5) and the option Show interference is quite handy when searching for duplicates.

I have been recommended to use Extracted Edges. ( Both GTAC and the Drafting Manual Best Practices.) I have not seen any up's or down's using this, apart from the benefits. ( Such as snapping sketches to those objects and opening "Structure Only".)


Tomas

 

[JohnRBaker]

'Optimal' is based on having views which look good, but since you appear to to be in desperate straits, I'm recommending that you forgo 'optimal' and try something which might provide at least some modicum of relief.

And for what it's worth, there are plans to work on Drafting performance as part of our next development cycle (but that does not mean the next version of NX as that code is all but done), even if it had not gotten the top vote at the recent Users Conference, however that vote should help us get the needed support from our management to commit the resources necessary to get as much improvement as is possible.

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]

It is disapointing that it has taken your management so very long to address Drafting performance; more disappointing is that we will not be seeing improvement until AFTER NX8.

Maybe by then the developers will find a better way to calculate the "optimal" value for chord tolerance?

Proud Member of the Reality-Based Community..

 

[BOPdesigner]

I was thinking of running a place view test on NX 8 (beta) tonight. But if nothing has changed maybe I won't bother. Toost thanks for the workarounds. I know there are a few tricks that can be done. The point is users should not have to mess around with such settings or spend additional effort preparing their model to place a quick drawing view all the time. Just drop a view and have it update and finish in 1 or maybe 5 minutes max (not a faceted representation). If you go into the roundtable discussion on plmworld.org you can find notes and slides of a discussion that was held back in Feb? on this issue:

http://www.plmworld.org/p/cm/ld/fid=36

Scroll down to the bottom. Thom9446, where can one find the results of the latest CIP on this? Were they revealed at PLMworld a couple of weeks ago?

 

[JohnRBaker]

The limitation is based to a great extent on the types of geometry needed to be included in a Drawing view so that things like Hidden-Line-Removal, selection of edges for annotation, creation of section views, etc work as expected. This is the area where we feel the maximum benefit can be achieved and it's where were are working at the moment.

Much of this requires that we make fundamental changes to the way so-called 'lightweight' representations of a model are stored and used by the system when displaying and interacting with models during a session of NX.

Anyone currently running NX 7.5, if you used the OOTB box settings, should have noticed that the display performance for assemblies, when working in many of the non-Drafting modules, is now much better. This is the result of work done at the very lowest levels of NX to assure that not only are we using the these lightweight representations for display of your models, but also that we can work with them in a manner such that you do not have to worry about whether you have an exact versus a 'lightweight' representation available when you need to perform some sore of in-context modeling operation. This is what we would like to have when working in a Drawing as well, being able to leverage as lightweight a representation as possible without having to fully load an exact model to perform everyday Drafting operations as mentioned above.

But getting back to what can be done today, as mentioned by Toost, not including every small or minor part in every view, particularly if you are performing a full hidden-line-removal (NO dashed hidden edges) on your Drawing views. To this end, the judicious use of the...

Assemblies -> Context Control -> Hide Components in View...

...can pay significant dividends when it comes to the time needed to compute the hidden-edge views of large and/or complex assemblies.

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 John. Glad to here there is an effort to address this. Hopefully I can keep the business from switching CAD systems between now and when we might see the benefit. Regarding Hide components in view. Aside from the simple cases (10 or less components I want to hide), I tend to shy away from that because if I ever need to go back and show those components again, it is very difficult to find the exact part I want to show (if there instances of the same hidden). So what I do is use layer masking (Visible in View) or most recently I used an assembly arrangement to suppress the components. Are these three techniques (hide component in view, layer masking - visible in view, and component suppression) equivalent in terms of impact on drawing view creation update time? I still don't think my question was answered regarding which assembly was larger in this regard. Few components with a lot of faces, or many components with a few faces. I suspect that it depends, but for drawing view creation (hidden line removal) it depends on faces/geometry more than on components, yes?

 

[JohnRBaker]

As long as you have sufficient memory so that you don't have to do a lot of swapping (already mentioned as an issue with 32-bit or any minimally configured system) it's the number and complexity of the faces which makes up the model that has the biggest impact. The actual number of components is not the primary concern, if they are all simple parts with only planar or cylindrical faces.

Another trick which might help, particularly if the view presented of your assembly is such that if everything 'behind' a certain point was 'hidden' that the Drawing view would still be valid, is to use clipping planes to virtually 'chop-ff' that portion of the model, normal to the axis of the view, which is not seen. To do this, select the view, press MB1, select 'Style' and open the tab titled 'Perspective'. Now set ONLY the 'Back Clipping' plane. Note that this could be a bit tricky as the distance is based on the center of bounding box for the assembly model. However, to give you an idea of what has been 'chopped-off', after enabling the clipping plane, you can 'Expand' the view and rotate it to see exactly where the 'clipping plane' did it's deed.

Another trick is that once a view has been set-up as desired and you're not going to be doing any additional work on it (adding annotations, doing some specific view-dependent editing, changing display options, creating detailed or section views, etc.) you can select the view and set it to be a 'Reference' view (this can be done from the General tab of the view Style dialog). Now even though 'Reference' views are not displayed when you open a drawing, they will be properly rendered when plotted or when a CGM/PDF file is created of the Drawing sheets. It's conceivable that you could set ALL your views to be 'Reference' and only toggle OFF that state for the views that you need to work on when you need to do so, meaning that you only 'pay' for an update when you change the 'Reference' status of a view making it visible again. Granted, this will not help the performance of the original view creation task, but once a view is created and it's not going to need any immediate work, making it a 'Reference' view can help in any subsequent updates that needs to be done as your placing or working with other views on the same drawing sheet.

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.

 

[Toost]

A bit late reply to this thread,
The problem with the proposed methods are that they can be done on a view that already has been placed, and then the HLR has already happened more or less.
We place the all the views on the sheet without update, ( Only the border is visible since no HLR has run.) then we start the update ( on 64 bit computers) when it is time to leave for the day.
When we come back we can then decide if we want to hide a component or not. ( and again take the update...)

 

[capnhook]

Sorta feels like the bad old days all over again, eh Toost? Thank you for the tip.

I wonder if the "man-year" has commenced yet, or whether it is all bulls#it....?

Proud Member of the Reality-Based Community..

 

[FLHTK]

Hello everyone, I just joined today. I have lurked here a couple of times in the past. I have had this View Placement/Update problem for quite a while. What we have found here where I work is: prior to placing a large view onto the Drawing Sheet, ensure that the Preferences-View-Hidden Lines-Interfering Solids is checked to NONE! This allowed us to place view in minutes as opposed to hours. Hope this helps.

 

[BOPdesigner]

I believe Interfering Solids set to None is the default setting.

 

[christian928]

Hi all, Very interested by this thread as I bought NX 7.5 this year to replace SolidWorks. I had been experiencing this problem, along with many many more, using Solidworks and I have seen a good improvement with the speed that NX updates drawings. NX can be slow, sometimes very, but Solidworks is definetly much slower with it's own native files.

One lesson I learned while working with drawings of large assemblies in SolidWorks was to keep the number of views to a minimum. Often I would create seperate drawing files and split the views up between them. This was a pain but better than losing most of my day waiting.

 

[NXrabbi]

I tried to read through all this to see if it was mentioned so I apologize if I missed it.
What about the Small Features options? This gives you a percentage factor which eliminates the display of any geometry smaller than that percentage of the overall geometry size. For physically large assemblies of perhaps several feet or larger, features smaller than an inch would be useless.
Another option that I am unsure of its impact on performance is Edges hidden by edges. If it's off, it's not displaying those edges in the back of the view that basically wouldn't show up anyway because of edges in front of them. But does that mean that it takes more time to process whether or not they are invisible? Or more time to generate those edges for the view?