Loading large catproducts in V5 R14???

[dtwo]

I am having problems with loading catproducts that contain a large number of catparts/catproducts. Some times it takes over an hour to load the data. I am a relatively new V5 user and looking for advice on how to dramatically reduce the amount of time to load "large" assemblies.

 

[Albigger]

Do you have "working with the cache system" enabled in the options?

I believe this mode just loads a graphical representation of all parts, then if you need to modify one part CATIA will just let you load that one part when you go to design mode.

I have not used it much, but it is supposed to cut down on load time. Maybe someone can clarify or expand on my statements.

--Jay

 

[DBezaire]

dtwo - As jay states you need to work with cache mode. Turn on this option in tools options infrastructure -- product infrastructure. There is another option to have on - load referenced documents, you can find this in tools options general page.
Your first load will be slow, Catia will make a CGR file (Catia graphical representation). Your next load will be fast and use low amounts of memory. When you double pick on a part, this will activate it (design mode). If you want to unload the part. In assembly mode, contextual menu, representation -- visualization mode. This will place the file back to cgr format. Note, while in cgr format the shading of the file when highlighted may appear like a triangle mesh, this is normal. If you update a file that has links to another, catia will load the associated files to the minimum level required to perform the update.
Hope this clarifies a few things for you

Regards,
Derek

 

[Kapmc]

dtwo:

Albigger is correct runnig in cache mode will greatly reduce the time it takes to open a file. But the cgr file has to be create first. The fist time you open a file with your cache mode turned on is when it creates the cgr file, this can take a while.

Also thier is one more option you can use, this is to turn off your "load reference documents" option.With this option turned off, only the 1st level products are shown,
you then can load any parts or products you wish to work on.

 

[Ataloss]

I know this will sound weird, but unplugging my network cable dramatically speeds up my loading of large assemblies in V5. I think it's the way IT set up my Catia though and because of my physical distance from the server. (Sorry, this gets a little long and is probably a very specific condition that few others will see).

Our design team is split up into three countries around the world, the US, France and China. There are approximately 40-50 designers in each country. We use Smarteam for CAD data management, and each country has its own server that syncs with the other two every 5 minutes to keep data current around the world. In the US we have two offices, our headquarters in California with about 40 designers and an office in Detroit (where I am) with 4 designers. The US Catia license server and Smarteam server are both in California. Acessing Smarteam through the Catia imbedded interface in Detroit does not work because the network connection is too slow, so we use a web-based interface that is separate from Catia. We do have access to all the company servers (Catia and non-Catia) through a WAN, so we are connected to our offices in California but the connection is slow (compared to being in California).

How I work is that I download data from Smarteam through the web, work locally on my laptop, and then upload it again when I'm done. Since I visit the customer I am able to pull a node-lock license for Catia and work when not connected to the network. What I found was that an assembly that would take about 10 minutes to load when in the office (connected to the network) would only take about 2 minutes to load when at the customer (not connected to the network). I did a back to back test at the office with my network cable plugged in and with it unplugged and verified the results.

I was shocked at the difference, so I started looking at settings in Catia. What I thought was happening was in Tools/Options/General/Document there is a setting for 'Linked Document Localization' that tells Catia where it can search for pointed documents (I think that's what it is for, at least). Smarteam is at the top of the list, followed by 'Folder of the pointing document' and 'Folder of the link'. I assume Catia is trying to search Smarteam for linked documents first so it tries to access the Smarteam server in California, times out, then starts searching locally. I explained the issue to our IT guy, but he is too busy to look into the problem because I've already found a work-around by unplugging the network cable. The setting is locked so I was not able to experiment and see if either disabling the 'Smarteam' setting or moving it so it had lower priority than 'Folder of the pointing document' or 'Folder of the link' made any difference.

Anyways, that's another possible suggestion for speeding up the connection. It is a rather specific set of conditions though, so it may not be of any help to you. If anyone has any suggestions about what is causing my slowdown, I'd love to hear it.

As others have said, using the cache helps a lot too.

Good luck,
Bob

 

[PeterGuy]

Linked document localisation is the search order that catia uses to locate linked documents. But the smarteam option defines that it should search your smarteam work directory for linked documents.

 

[flangewiper]

We have the same problem and generally find the following works well.

1. Put the kettle on

2. Make yourself a cuppa

3. Put your feet up and wait.

It doesn't get the job done any quicker but big products will always take time to load even with cache mode turned on.

 

[Ataloss]

Thanks for the explanation PeterGuy.

Bob