SE causing long waiting times (SE V15) 1

[SolidEd]

We are currently having problems with the amount of time it takes to open, save, close, even minimize and maximize files (literally minutes for moderately sized files). This is a problem that has been here since I've been here. Up to this point it had been thought that our hardware configurations were the culprits so we have spent time and money upgrading our systerms (not very top notch, but none the less much better than before) with little success.

I recently did some tests where I found that if I copy the files and linked assemblies to the local drive (c, wait time goes from minutes, to mere seconds. We then ran perfmon on the server (dedicated server for our files) to see if we could spot the problem (hd, network, etc...). What we found is that Processor and hard drive activity are realtively low but there is a lot of information being transfered over the network even when we simply minimize an already open drawing (causing the long wait times). Network speed, CPU, HD, RAM do not appar to be factors. Why is SE transfering info here? What can I do to minimize this wait time.

Any helpful information related to this topic would be greatly appreciated.

Thanks in advance

 

[Alwinus]

What kind of serversoftware ar you using? I've learned that SE is not so good with Linux(Samba). Windows should not be a problem...

 

[roblom]

We've had the same problem. We upgraded to a 1 gbit network connection with succes.
I don't know why SE is transferring so much information over the network but it's cousing a lot of waiting.
A PDM program may be the solution because then SE copies the files to the local drive.

 

[SolidEd]

using a Windows 2000 server, raid 1

OK, we hooked up a packet sniffer between my pc and the sesrver and basically, when I open a 2D drawing, solid edge is opening every assembly and subassembly linked to that drawing, down to individual parts like bolts and screws. So for instance, a 6MB 2D drawing I was using for tests, that shows one small piece/part of our machine is made from a view of the machine model. By opening the drawing, it is then going out and opening the machine model that is linked to it. It is then opening every sub assembly that makes up the entire machine down to nuts, bolts, washers, etc... so this 6 MB file winds up bringing 100's of MB's with it. The most puzzling part is that if I have two drawings open at the same time, it does the same thing when simply changing focus from one drawing to another (solidedge closes all the parts, assemblies and subassemblies of one drawing and opens all for the other).

BTW, the tests I mentioned above that pointed to a netwrok problem (where copying the files locally worked much faster) is wrong and void since although I did copy the main assemblies linked to the drawing I didn't copy sub assemblies, screws, individual parts, etc... I placed the same files I had copied to my local drive on the network and received similar times as when I open them locally. The packet sniffer showed that it actually looks for all the individual parts and sub assemblies but simply moves on when it can't find them, causing a much shorter waiting time to open.

 

[SolidEd]

now that I think about it, we've also been having a problem with the explode feature. Every time we try to explode an assembly, instead of just pulling the sub assemblies appart, it explodes every fricking component apart. I wonder is this is somehow related.

 

[Kenny_G]

SolidEd,
That is how the explode command works. If you do not want the subs exploded, you must use the "Bind" command and select all the subs that are not to be exploded.

Ken

 

[Kenny_G]

SolidEd,
If upgrading is an option, you may want to think about it. I believe V16 introduced a new behavior were it only accessed model data from the drafts as it was truly needed. Of course, I can't say I've ever experienced issues like yours before. By the way, V18 is the way to goif you do decide to upgrade.

Ken

 

[SolidEd]

Upgrading would be ideal. I just need to justify the cost in terms of new features (that benefit us) and some of these problems being fixed.

 

[beachcomber]

SolidEd,

So for instance, a 6MB 2D drawing I was using for tests, that shows one small piece/part of our machine is made from a view of the machine model

If I have interpreted the statement correctly, it could explain why you are having problems.
Are you saying that you create drawings of parts and sub-assemblies from your main assembly, or was that just for a test ?
It's true that SE (up to V15) has to reference all the parts in an assembly when opening or switching between drawings - it's how it checks for out-of-date parts- and also when switching from model to drawing.
That's why you should create the drawing from the 'smallest' model.
I can't say if V16 etc has improved the problem.

bc

 

[donyoung]

Hi @all,

with V17/Sp6:

- opening a draft still accesses all parts in the assy (just to check
on any outdated items)

- double clicking on the view to see the model obviously fetches
all the parts

- switching the window to/from any other draft already opened does
not result in any recognizable disk activity

dy

 

[SolidEd]

beachcomber, your interpretation is correct. We make most of our 2D drawings from views of the assemblies. Obviously, when the drawing is only of a part or a sub-assembly, then we only use their models and not a model from an entire assembly. however, in the test mentioned above, the drawing is to show how a certain part is assembled into a certain section of the machine, so the entire machine model was used. This is very common for us to do. Is there a better/different way of doing it aside from turning the view into drafting views (which would then disconnect the association from the model)?

Donyoung, thanks for the info. I can deal with the opening/saving/closing times, it's the time it takes to switch from one open drawing to another that just drives me crazy.

 

[beachcomber]

SolidEd,

I picked these tips out of

http://www.solidedgecommunity.com

for improving speed and efficiency of Drawing Creation :-

Place drawing views with all options for hidden lines switched off.

"Display Configurations" should be created in the assembly environment and used in drafting for view creation.

Use "Simplified Parts" and "Simpified Assemblies" for view creation wherever possible.

Only link one model file (PAR/ASM) to one drawing (DFT). This reduces the amount of file searching that has to be done.

Working on large draft files should be done locally.

Once the required views have been created in the draft file, use "Reduce File".

My last Solid Edge job involved working on assemblies with 18000+ parts .
For the top-level assembly drawings we put one view per file wherever possible, and I created view configurations showing the minimum number of parts required for each view. To help with this I used the "select visible parts" command and then used "show only".
It's a great way of reducing the amount of data to be processed. I reduced one drawing from an impossible-to-work-with 120MB to about 40 or 50 MB.
You can do a similar thing for section views - by hiding all the parts you know will be in front of the section plane.

bc