component substitution in NX5 verrry slow!!! 1

[scope63]

hi

due to engineering changes i am finding that it takes hours to substitute a component in NX5. the component that is being substituted is rather larger in size (220Mb). i am running a 64 bit dual processor computer. it takes over the computer completely and does not let me do anything else.does any one or has any one run into this, and have a solution?

Scott Copeland
Mould Designer
G-Mag International Inc

http://www.g-mag.ca

 

[hudson888]

It is likely to be slowing down because you're stretching the amount of available memory to near its limits.

First I think you'll want partial loading turned on in your load options.

To limit the amount of memory you're using to begin with try using faceted representations and setting your default reference set to the faceted one, (i.e. often called REP or FACET). This can also be found in your load options.

When stuck on these kinds of things try doing the manual equivalent. When you substitute a component the system seemingly tries to open it fully I guess to check for any dependencies. Operators often already know this won't be necessary although the computer of course cannot be certain unless it checks. By going manual I mean delete the component and then add in the alternative as two separate operations. This is where the partial loading will also help because you should be able to select the reference set of the component you're adding to be the Faceted one or even Empty by following the add component dialogs. How partial loading works is that it adds into memory only the part information it needs rather than the full 220Mb.

Other things that could we in the mix are a lot of wave links and mating conditions. If you do what I described you'll quite likely lose all of the associations. On the other hand if there were so many that to express them all you need to load more geometry than the computer can handle then you need to question their value. I know some people don't like hearing that, but if you don't look at some ways of working more efficiently you can find it very hard to maintain your data.

Sometimes using Teamcenter in these kinds of cases imposes an extra overhead with maintaining the database. However few Teamcenter users are able to quote the file size as 220mb so I'm guessing this isn't you.

let me know if I've made some wrong guesses here and how you go with your problem.

Cheers

Hudson

 

[scope63]

the unfortunate thing is the part i'm trying to substitute is the customer model. i need to extract faces and regions to build up my mould parting lines so i need almost all of the geometry active, unless you are telling me that by loading partially i can still use these faces. i did try once with a model that i got and found that the format was set to facet and i could not select anything to make any changes until i set for example model in the format.

thanks for your response.

Scott Copeland
Mould Designer
G-Mag International Inc

http://www.g-mag.ca

 

[hudson888]

From what you describe you have your customer model in an assembly presumably with some other components. By using partial loading and representations you will be loading very little of the component geometry on demand when you first open your assembly. When you change reference sets to Solid then you'll be loading more, but you can sneak up on extracting geometry bit by bit until you have the full compliment of what you need.

In order to set this up manually on existing parts you would need to be able to create Faceted Representations and I think you may need an Advanced Assemblies License for that. Most people set up their customer defaults to create them automatically under Utilities>Customer defaults>Assemblies>Site Standards there is a Representations Tab where those settings can be made. Once done the system will create a reference set containing the faceted bodies regardless of the License. You would need to make the change restart NX and then reopen and save any older parts to effect the changes fully.

After that you look into your load options turning partial loading on, and setting the default reference set to the name you have chosen for your faceted representations. In NX-5 you can just move "use lightweight" to the top of the priority list, if your customer defaults are set as described above. The next assembly you open will be as lightweight, and that will start to save you time.

Do one other thing if necessary turn off "load interpart data" under your load options and turn on "Delay Interpart" under Tools>Update. This limits the effect that wave links will have on opening interpart data. It also means that the process of keeping wave geometry up to date is less automatic. You may want to change those setting later or when working on smaller less demanding assemblies, but for the moment lets get you every bit of memory we can claw back.

With extracting geometry from a customer model we would most likely use wave links initially, but we often try to lighten the load and keep it simple by breaking the links after the geometry is extracted. One reason for this is that if the extracted data describes an interface from a customer model that may later be updated then you often can't rely on updated versions to contain the same number of elements so chances are the model would fall apart in the process of trying to automatically update. Better in that case to make the process more manual, and indeed broken links can be manually recreated as required so why waste time having the model attempt to check and rebuild itself whenever you preform an "update session".

Anyway see how you go based on that info, and please get back to us if you think it has helped.

Cheers

Hudson