Un workable assemblies

[Ian01]

I have a problem with SW assemblies which I ca't seems to shake.

My system is up to spec, so I know its not that and this problem was seen on the upgrade to 2003.

I use small assemblies but they are all parts which are generate from the first one in the tree. Making moulds using mainly the Cavity Tool. The Cutting and extruding where required. At a certain level in the assembly SW seems to want to rebuilt every single feature in every single part within the assembly, even parts which are not linked to a change or an addition.

The problem is that severe, to drop a part in an assembly can take 2 mins, and rebuilts range from 15-20 mins.

Getting so bad the assembly becomes unworkable. The last resort is to parasolid the assembly. hence losing my tree but allows me to work on the assembly.

any ideas anyone, and please its not hardware.

 

[SBaugh]

Are you working over a network?

If so have you tried coping to your Harddrive and seeing if you get the same result?

If you get the same result on your HDD, then you should look at either the software, the hardware, or the way the model is designed (complexity)

If not, then your bottle neck is in your Network some how.

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
When in doubt, always check the help

 

[Standing]

Make sure that your System Options – Backups settings are set the way you want them. I have Unchecked the “Save auto recover info every 0 changes”. Use Ctrl S when wanting to save. Uncheck “Save backup files in the same location as the original”. Save backup copies in directory: “C:\swSolidWorksBackups” is just an opinion.
Also in System Options – Large Assembly Mode Uncheck “Save auto recover info every 0 changes”.
Also in System Options – Performance, Uncheck Verification on rebuild. Use Ctrl Q when wanting rebuild.
This may not be your problem, but it is worth giving a try. No loss in performance, and not a lot of time to check out.
When we were starting SolidWorks several of our users had “Save auto recover info every 1 changes”. On some assemblies this caused a lot of confusion. Until we found out why.


Bradley

 

[MadMango]

I'll add to this, to check the complexity or "level of detail" of your components. Suppress helix-based features, fillets, etc of parts that are not visible.

If you have compnents in your assembly that will not change, consider saving them as Parasolids and make them SLDPRTs again. Many of the compnents I work with are COTS (commercial off the shelf) and don't require a parametric model. I "dumb" them down via the parasolid route, and my rebuild times drop from 2-4 secs to less that .50 secs per part. That time adds up quickly when I'm working in an assembly of 500-700 parts, or more.

Ray Reynolds
Senior Designer
Read: faq731-376
"Probable impossibilities are to be preferred to improbable possibilities."

 

[macPT]

Something like that already hapenned to me!

After some unsuccessful tests I reinstall SW... and the problem remains. I started to think: reinstall OS (horror!).

Before I do that one last test: tools/options/file locations/referenced documents and I add the exact path for the assembly. Everything work fine!

So, what was the problem? The files are currently on folders on the network. I have the referenced documents option pointing to these folders. I have moved the assembly to the local disk. I think that, for each component, SW was trying to find the file on the network before searching the local disk. If I had the computer disconected from network, this assembly was unusable because it take about 1hour to retrieve!

Now I allways change this option adding the folders that I am currently working. That speeds up a lot retreaving files (and I mean A LOT!).

Good Luck

 

[Standing]

When one wants to copy an assembly to their hard drive to test opening speed, comparing opening on a network. Use File, Find References…, do not Preserve directory structure? . Even using this method, I have seen SolidWorks remember a few locations scattered on the network (I mean very few, say 1 out of 3000).

Bradley

 

[macPT]

Bradley

I agree with you. It's very risky to use that method. The safest method I now is copy to the local disk and disconect from network.

Surprises hapen now and then.

Regards

 

[StarrRider]

macPT

I have always used a network mapped drive. When I want to see if the problem is net related, I simply dump all of the files into one directory on my system and remove the mapped drive. The network is still hooked up and useable, but SW will be looking for a drive that isn't there.

Since SW always checks the active directory when it is opening files, you don't even have to change the links where all those files came from. SW will open the files without a hitch. Further, if I did miss something, I can still use Windows Explorer to get it and dump it into my working directory and then find it.

If you have room to copy all of the files from your network onto your local system and want to maintain the correct paths in the assembly file, you can recreate the directory structure with a CMD file that contains a Subst command. I use this little trick so that I can duplicate our network drive on my home system where I do not have a network.

As an example: If your network directory is mapped to Drive X, copy all of the files into a “DriveX” directory on your C Drive. Then create a CMD file that contains the line
Subst X: C:\DriveX

When you double click the CMD file, it will create an X Drive that looks identical to your network mapped drive.

Lee

According to an unfinished survey - 9 out of 10 people . . . . .

 

[macPT]

StarrRider

When you say "... SW always checks the active directory...", I think you are correct, but I think there are two "problems" (they are not realy problems, but we need to remind this so we don't have surprises):
1- if you did not hide the original directory (using your suggested methods, for example) SW will retrieve the files in the original directory, ignoring the files on the active directory. If you made a copy to test alternate design solutions, you are in fact modifying the original files.
2- if you did hide the original directory and the active directory is not difined in the Options/file locations, the active directory will be the last where SW search for the files (the first are, I think, those in SW options). That's why it can take a long time to open assemblies, but it will open. The pratical result is that, in some cases, it can take so long that we can consider the assembly unusable.

Your methods are OK (by the way, does Subst CMD works on W2K?). I normaly disconnect the network cable (just for sure!) and temporary define the active directory in SW options.

I need this mainly for 2 reasons:
1- as I already mention, for alternate design tests (before decide to modify the design)
2- to simplify parts and assemblies for FEA purposes.

Regards

 

[StarrRider]

macPT

You are right on #1 – The mapped drive defiantly has to be removed before you local directory is even looked at.
For #2 – The only directories that I ever have in the Options/File Locations are mapped directories. This causes problems for me because my templates are on my X drive and when I don’t have one (because I didn’t hit the CMD file) SW wants to remove those settings. It prompts you before it does it, but one of these days my fingers will be faster than my head and I’ll have to reset them.
As for the speed – I have never noticed this as being particularly slow. I have seen a lot of things slow SW down to a crawl, but this is not one of them.
I have a question for you though. I assume from what you said that you are have several directories for storing your assembly files and those directories are listed in Options/File Locations/Referenced Documents. Why are you doing that?

Yes it does. I was using Subst in NT originally, when I upgraded my home system to Win2k it still worked. It also works on my laptop - which has XP\Home.

I do have to warn you though that I tried using it at work and it turned into a royal nightmare. We were new to SW then and had all kinds of file locking problems. So I copied everything to my hard and worked on a project for a month. Several other users saw what I was doing and did it too. The next thing I knew, someone was overwriting someone else’s files every time we turned around.
Now, I do it primarily so I can take an assembly home and work on it. Occasionally, I still do it when I have a lot of common parts to add to a large assembly and have to do a lot of mating. I copy everything to my hard, but I only copy the assembly I’m working on back up onto the network. If I do have to changes to any of the other file, I keep a list of the files I changed and only copy them. It works for me.

Lee

Who is the most popular guy at a nude beach?
The guy who can carry 7 donuts and 2 cups of hot coffee!
Who is the most popular girl at a nude beach?
The girl who can eat all 7 donuts!

 

[macPT]

StarrRider

We don't have mapped drives in SW Options/File locations/Referenced Documents. We configured these options clicking Options/File locations/Referenced Documents/Add/Network Neighbourhood/... and then browse to the intended folder. This will create a link in the form \\hostname\folder\... and you don't need to have a mapped drive.

The reason to do define these options is that we have one folder for all the parts, assemblies and drawings for current production (only the latest versions), another for components (screws, washers, motors,... everything we buy to incorporate in our products) and some other folders (variable) of new products currently in design process. When a new design is successfuly ended, the drawings are issued for production and are moved, with parts and assemblies, to the first folder (using MSExplorer). In these folders (except for the components folder) we can share components (for example, in a new design I can use screws alredy used in other products, or even use parts or assemblies already in production). So the only way we have to easely manage these files location and moving them using MSExplorer is telling SW where to look for them, as the expected folder as disapeared. This also speeds retrieving.

It is forbidden to the other users to save files in folders other than those I have discribed. I am the only one who can do that and only in the referred special cases (and also to take some work home). This is the result of the same problem you described. Now we don't have problems regarding file management.

Regards

 

[SBaugh]

If you want to see how SW looks for files check out this KB article at the SW website. You have log into the Subscription services to view it. ID #72428

Best Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
When in doubt, always check the help

 

[StarrRider]

macPT

I believe we were doing most of that with mapped drives. We started using them when one of our servers died and the new server ended up with a new name in our directory structure. We mapped Drive X to our current projects, Drive Y to production files, and Drive Z to purchased parts.
In the X drive, all parts and drawings are stored in a single directory with the exception of purchased parts - which we always placed where they belong on the Z drive when created – even if they never get used.
When a project is finished, a Product directory is created on the Y drive and the TLA (Top Level Assembly) gets moved into it. We normally have 5 or 6 parts with every project that are product specific. All of the other Parts and Drawings get dumped into one of our Production directory – all part number files beginning with 123 go into the 123 directory.
I too get blessed with the honor of making the move. All of the files are moved with MS Explorer and the Project directory is deleted. Then every assembly is opened and the file locations are resolved. This doesn’t take as long as you might think. With a new product, nearly all of the parts and subassemblies end up located in the same directory and only a single lookup is required per assembly. This is fairly easy now but it was a major pain when all of the purchased parts had to be properly put away. The drawings also have to be opened, but because they are in the same directory as the parts or models, it becomes simple. I get a file not found, find it prompt – Yes – Select file dialog & hit enter.

After reading Scott’s link, I think that if you are experiencing extremely slow assembly opens – the reason for it is the number of places your making SW look for your files. Since it checks every one of the directories in the Options/File Locations first, the more directories you have in there the longer each new project is going to take.

Lee

According to an unfinished survey - 9 out of 10 people . . . . .

 

[macPT]

StarrRider

I have read it too and it turns out like I supected.

But I fill confortable with this with our process and I'll continue to use it: if I make a local copy, I will difine this local copy in SW options (bringing it up).

I seems to me that we have a very similar file management process. The only "big" difference is that we don't use mapped drives.

Regards

 

[JNR]

You know me, the K.I.S.S. guy. Here is a general speed tip which will amaze you. If you are running on Win XP go to Settings, Control Panel, System, Advanced, Performance (visual effects....) and turn off everthing except the fourth from last and the last one. (If I recall correctly that is "Use background image for each folder type" - doesn't seem to hurt anything and it's nice - and "Use visual styles in Windows and Buttons" - which gives the basic XP look as opposed to a Win 2000 look). Who needs to have their CPU constantly computing shadows for the cursor arrows, for example?!!!

You will be amazed at the speed increase in every application, not just SolidWorks. All that sliding and fading, etc. takes a huge overhead (apparently much more than it should).