Very slow processes on NX 6 - 7.5

[Ekide]

Hi everyone,

We are having a consistent performance issue while doing some very simple tasks on NX6 and NX7.5 on every workstation we have.

A such simple task as copying a whole assembly into a new layer takes this time:

* NX 6 ---> 41s
* NX 7.5 ---> 75s

We have tried the same procedure with the same assembly with these factors toggled:

* Autotune enabled/disabled.
* Workstation FW enabled/disabled.
* License server enabled disabled.
* Changed from licenseServer1 to licenseServer2

On every scenario the result is above 40s on NX6 and above 72s on NX7.5.

We have tried a "trial" copy of NX7.5 and completes almost instantly (less than 2-3sec) these tasks on any workstation we try.

Any kind of help would be much appreciated.

Thanks in advance,

--Iñaki Quintanilla Campos

 

[looslib]

What OS are you running?
How much RAM in the workstations?
What is the EXACT version/MP of NX?
Are you running the proper version of NX for your OS (32-bit on 32-bit OS, 64-bit on 64-bit OS)?

Copying an assembly between layers??? In NX your assembly should just be pointers back to the component files. Are you grabbing all the group (and hidden) data associated with the components?



"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[jpetach]

Ekide,

In addition to the points that Ben made -

and based on the statement
"We have tried a "trial" copy of NX7.5 and completes almost instantly (less than 2-3sec) these tasks on any workstation we try.
"

Use "Help-> NX Log File" on your machine and on the trial installation immediately after launching a fresh NX session and look for differences in the directory paths. Check for network shared drives especially for locations for temporary files.

Also examine which customer .dpv files are being used in the respective sessions and look for differences in the settings (or use "file->utilities->customer defaults->manage current settings")

HTH, Joe

 

[Ekide]

I'll try to answer as much as I can (out of the office atm).

For Ben:
*What OS are you running? W7 SP1 64bit
*How much RAM in the workstations? 12GB
*What is the EXACT version/MP of NX? problem happens from 6.0 to 6.0.5.3 and from 7.5 to 7.5.5.4 afaik. On the other hand NX 4 on the same machines works fine and completes every task in a flawless period.
*Are you running the proper version of NX for your OS (32-bit on 32-bit OS, 64-bit on 64-bit OS)? yes, its the 64 bit version.


Please keep in mind that they're fairly new installations on some decent certified Dell Precision Workstations and this problem is present on every machine.

The copying an assembly between layers is just a proof test that lets us know something is not working fine. I have back in the office a couple of tests more we usually make to make sure everything is not messed up. On this test the complete model is located on a local folder into the workstation.

For Joe:

The location for temporary files is forced to a local folder with full permissions on the user.

I'll have a look on the log file asap. Same with .dpv.

Thank you both for your fast response. Don't hesitate to ask for more info.

--Iñaki Quintanilla Campos

 

[Ekide]

Hi,

I have tried with another process and the time to compute is still too high.

I just cut a section of the whole assembly. Always the same section.

On NX4 it takes 1s
On NX6.5 it takes 1-2s (still reasonable)
On NX7.5 35s with autotune disabled, 37s enabled.

I'm attaching the assembly we are using as a test. In case anyone could see any big mistake on it.

Please feel free to criticize anything on it.

--Iñaki Quintanilla Campos

 

[Arkance/PhoeNX]

Section as View -> Section or as in trimming all the bodies by a plane?

Anthony Galante
Technical Resource Coordinator

NX4.0.4MP10, NX5.0.6, NX6.0.5, NX7.0.1, NX7.5.0-> NX7.5.5 & NX8.0.0 -> NX8.0.1

 

[Ekide]

Trimming all the bodies by a plane. We are aware that this way is much slower, but it takes a ridiculous amount of time.


--Iñaki Quintanilla Campos

 

[Arkance/PhoeNX]

I tested your sample part in NX4 and NX7.5.
In NX4 if I select all bodies (over 2000) the trim bodies to plane does not work as most of the bodies do not intersect the trimming plane.
In NX7.5 if I select the same bodies, the trim operation does take a long time (approx 60 secs). But the trim does work and you get an alert saying that some bodies do not intersect the trim plane.

On the other hand, if you sew the 1997 sheet bodies into one solid, the trim operation works much quicker. In NX7.5 there is a preview of the result so if you turn that off it's the same time as NX4 with the same geometry.
Why you are working with sheet bodies for what should be a solid object? The section test is flawed because of the number of sheet bodies.

As for the copying to layers in my testing NX4 is quicker than NX7.5. My thought is that when NX is doing the copy it is also generating the lightweight representation at the same time. I might be wrong but in NX4 I dont't believe this occurs automatically and would explain why it is quicker.

Anthony Galante
Technical Resource Coordinator

NX4.0.4MP10, NX5.0.6, NX6.0.5, NX7.0.1, NX7.5.0-> NX7.5.5 & NX8.0.0 -> NX8.0.1

 

[Ekide]

Hi Anthony,

Many thanks for all your thoughts. They've been really helpful.

**Why you are working with sheet bodies for what should be a solid object?

I'll have a chat with the design team on this issue, as it seems practical to create a single body. But it might not be feasible on their current job operation.

Regards,

--Iñaki Quintanilla Campos

 

[Arkance/PhoeNX]

It might not be feasible to create the model as a solid (my guess is the sheet bodeis were imported from another package), but once the surfacing is complete, Insert -> Combine -> Sew will knit those sheet bodies into one solid if they knit with no holes. Your example does that just fine.
I would also advise using Insert -> Synchronous Modeling -> Optimize -> Optimize Face, to clean up thae faces and edges in the solid.

Anthony Galante
Technical Resource Coordinator

NX4.0.4MP10, NX5.0.6, NX6.0.5, NX7.0.1, NX7.5.0-> NX7.5.5 & NX8.0.0 -> NX8.0.1

 

[Ekide]

Hi again,

I've tried both procedures:

**Insert -> Combine -> Sew
This one doesn't work properly as I apply it. I just get a bunch of alerts telling me that its not possible to sew that part. My fault I guess.


**Insert -> Synchronous Modeling -> Optimize -> Optimize Face
It does fine but it just removes 20-30 items from a 4000 item list.

So no improvement so far.

Thanks anyway, they were quite good ideas.

--Iñaki Quintanilla Campos

 

[Arkance/PhoeNX]

I have created a video of sewing the sheets & optimising the faces of that new solid.
The file is over 700Mb so I used Winrar to compress it. Google winrar and you will find where to download it to uncompress the two files. The other file is the new version of your original NX part.

Also had problems uploading the files to eng-tips so I have put them on our sharefile site:

https://phoenxplm.sharefile.com/d/s37ab898ec4c4a6db

The files will only be available for 7 days.


Anthony Galante
Technical Resource Coordinator

NX4.0.4MP10, NX5.0.6, NX6.0.5, NX7.0.1, NX7.5.0-> NX7.5.5 & NX8.0.0 -> NX8.0.1

 

[Ekide]

Wow,

That is just impressive. Many thanks for the video.

I'll have it in mind when testing. Unfortunately I don't have access to the CAD workstation until monday morning.

I'll update on the issue then.

Regards,

--Iñaki Quintanilla Campos

 

[Ekide]

In response to Anthony,

I have tried it on our local workstations and it seems a huge improvement from where we were. Now it seems more a design team task to work that way or the way they used to before.

A few questions arise on the subject, not from me, but from the design team:

* Can we say that the over 70 sec mark is a normal time for an assembly with so many parts on those operations I suggested (trimming all the bodies, copying to another layer, etc...)?

* Does this time have to significantly change among NX versions or license types?

They might sound obvious for you but I wanted to make clear I have understood them correctly.

Thanks again, all the IT department here thinks that the video you posted is an impressive piece of help.

--Iñaki Quintanilla Campos

 

[Arkance/PhoeNX]

1. The time doesn't seem unreasonable. But it would depend on the computer, version of NX, type of geometry.
2. License type would have no bearing on the time taken. The versinof NX would, but as I explained I think the variation between NX4 and later versions is the automated light weight representation creation.

Anthony Galante
Technical Resource Coordinator

NX4.0.4MP10, NX5.0.6, NX6.0.5, NX7.0.1, NX7.5.0-> NX7.5.5 & NX8.0.0 -> NX8.0.1

 

[Ekide]

Many thanks again.

I¡ll forward all this information to the design team. And with all in mind look forward to a better and faster way of work.

Thanks,

--Iñaki Quintanilla Campos