77 MB Top Level Assembly and Drawing SLOWWWWW

[ptc-3365282]

PTC!!! I have a huge assembly open with drawing, help me speed this thing up. It takes 30 minutes to open on a high speed connection.

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[BenLoosli]

Use simplified reps.

Does the model have lots of complex geometry?

How many components are in the assembly?

Are all the files saved in the current version of Creo(Wildfire)?

Are you using a PDM system or native filing?

[bsuslowicz]

Marty,

We had similar issues years ago but have since upgraded to Windchill, creo2 and got new workstations so now are able to open very large models. I don't know if it's one thing or the combination that helped.

I just checked one of my large assemblies, 101MB with 823 objects. It opened in under a minute. Even bringing into a new workspace and opening direct from Windchill took less than 2 minutes.

Are you opening it direct from the server or is it stored on your machine? If from the server, can you save it to your machine and try opening it? If it opens a lot faster, it sounds like a network issue. If no difference, it's most likely your workstation or the model itself.

Simplified reps will help once you open the model but will not help the initial opening of the assembly.

Complex geometry, especially rounded surfaces will greatly slow down the regeneration but you will see this slowdown every time it regenerates.

How the parts are created (features used) and how they are constrained in an assembly all make a difference. You could try openning lower level sub-assemblies and parts to see if one or more are much slower than others.

Let us know how it goes.

Bill

[ptc-3365282]

We pull the license from the network, I copied it to my desktop on my computer an it still runs slow. We are a large company with large models. There has got to be a setting or something. I have done everything, I mean EVERYTHING. Everything you have told me I have done. I just don't think the program can handle all of this information. I am pulling the license off of the network.

[bsuslowicz]

You said you pulled the license from the server, can you download the assembly model and parts to your workstation so you don't open it across the network?

[ptc-3365282]

Use simplified reps.-yes

Does the model have lots of complex geometry?-yes

How many components are in the assembly? a ton

Are all the files saved in the current version of Creo(Wildfire)?yes

Are you using a PDM system or native filing? no native foling to a folder on my desktop

[ptc-3365282]

Use simplified reps.-yes

Does the model have lots of complex geometry?-yes

How many components are in the assembly? a ton

Are all the files saved in the current version of Creo(Wildfire)?yes

Are you using a PDM system or native filing? no native foling to a folder on my desktop

[ptc-3365282]

I even turned off automatic regeneration and the program is lagging very bad. like 30 minutes to an hour.

[dschenken]

If only the model is opened without the drawing - is that fast?

1) try going through the assembly and suppressing items - say the last 50% of the components. Is it still slow?

2) repeat step 2 until it is fast

3) resume everything

4) in the last segment that was suppressed, divide that in half; repeating this process will locate any problem parts.

Look in the trail file for the assembly for Warnings that you don't expect. It's probably a big file so it may take a while.

Check the accuracy of the parts - if it is very small it may be increasing the memory and processing required.

Check to see if you have the latest drivers for your graphics card or roll back to an earlier driver version. Newer is not always better

What is the graphics Config option setting?

I see nothing about the config of your computer. If your usage exceeds the amount of physical RAM in the machine, or even comes close, the software will page to the hard drive - which is approximate 100 to 1000 times slower than if it remained in RAM. You can either get more RAM or try setting up an SSD instead of a hard drive. This will move the slow interface to only 10 to 100 times slower.

[dschenken]

101MB - was that size on disk? Because that has no direct relation to size in memory or complexity of graphics. If models have been stored with high resolution previews, those can get very large for not much resulting model in memory.

[bsuslowicz]

David,

101MB was the total size of the workspace with assembly, part and drawing files. I only listed it as a comparison to Marty’s 77MB file.

I agree that total size has nothing to do with memory requirement or graphics complexity.

[TomU]

Marty,

Where you pull the license file will have zero impact on the performance. Where you run Creo from (network or local installation) will have almost zero impact on it's performance. Just to prove this, borrow a license. You can then physically disconnect your network cable and Creo will still run. See if you notice any change in performance. I'm pretty sure you won't.

[ptc-3365282]

Borrow a license? We are a big company I cannot be messing with the license

[TomU]

To borrow a license you just use a different shortcut to start up Creo. It's not hard or dangerous and shouldn't require help from IT or anyone else. Is Creo installed locally on your computer?

[ptc-3365282]

Ahhhh....no it is not...hmmm I think you may have hit the nail on the head. We open it from a company menu.

[ptc-3365282]

It's a floating license

[ptc-3365282]

You know, the assembly doesn't take long to open up, it's the 14 sheet drawing. It's to bad creo makes you open all of the sheets at once in tabs in one session.

[dschenken]

You can create drawing configs that have all the views erased and just resume the views you are working on - this is handled by a drawing Representation.

See http://help.ptc.com/creo_hc/creo30_pma_hc/usascii/index.html#page/pma/detail/To_Configure_a_Drawing_Representation.html

and

See http://help.ptc.com/creo_hc/creo30_pma_hc/usascii/index.html#page/pma/detail/Default_Drawing_Representations.html

[ptc-3365282]

I see that, but man that sucks too. PTC just needs to make it faster then all my problems would be solved. ha Whole lot of up front configurations.

[ClintWalton · Accepted solution]

Hi Marty,

There are quite a few available documents discussing performance improvement settings for both large assemblies (assembly mode) and drawings containing large assemblies. Here is the best one to start with:

http://support.ptc.com/cs/cs_27/howto/vew1046/vew1046.htm

[ptc-3365282]

Ugh, this is still a lot of work PTC. but thanks for the info I will just make do.