odd toolbox behavior 1

[dsgnr1]

Does anyone else ever get this kind of behavior from ToolBox?

I grab a 8-32phms from the TB and it reports "pan head Cross_ai is already opened. Do you want to show the open file"?

I select yes, then drop the toolbox part on its default ref mate and check the green check confirming the correct TB part. Then Solidworks assembly zooms itself to extents and thats the end of that TB session (no repeat drop). then I must start the same thing over again if I don't want to pattern.

Working over a shared network with 4 or 5 other users. Toolbox gives the green light for being set up properly. Not all hardware acts this way. Some hardware drops in and keeps going.

just curious if anyone else has seen this and if there is a fix.
thanks,

¿)
Version of SolidWorks: 2009
SolidWorks Sercive Pack:sp3
Operating System & Service Pack: winxp pro v5.1 (sp2)
Graphics Card and Driver version: Nvidia Quadro fx540, 9.1.3.6
Amount of installed RAM: 3GB
Virtual Memory settings: APPS, total paging = 1024mb
CPU Type & Speed: intel pent 4 / cpu 3.00GHz

 

[Waidesworld]

What we did, and I know it wasn't the best practice, was get one of our techs to grab all the screws, nuts bolts etc that we use from the tool box. He then renamed them and saved them in our nuts-n-bolts folder. It eliminates some of the smart fastener features but in reality we are too small to use it as it should be done.

drawn to design, designed to draw

 

[rgrayclamps]

Hi, dsgnr1:

This behavior is not odd. It happens when:

1) The assembly you worked on (or another assembly opened in background) already contains a reference to another Toolbox different from the one you are tring to use;

2) You opened an assembly containing toolbox items from another toolbox, and you did fully close it (i.e, the other toolbox still resides in your computer RAM);

3) The item you try to insert into your assembly did not have read-only atribute.

If you launch a fresh session of SW application and open a new assembly document, you will not see this message when you insert toolbox items.

Good luck!

Alex

 

[dsgnr1]

thanks for the replies. I will check on the items that you listed. I have seen another location on root, but didn't think it would matter since there is no db there. And sw is not pointing to it. I got a systems admin that is really good, so he can help me sort this out the rest of the way.

We don't wanna use the vault room for each pc of hdwr, so making parts is out. One thing I wish I had forseen when we started using toolbox (2001i) is that we shoulda' just left our in-house part numbers out of it and printed a sheet for the floor to equate, i.e., phms 8-32 x 3/8 = 64a0091/06. Lesson learned there.

¿)
Version of SolidWorks: 2009
SolidWorks Sercive Pack:sp3
Operating System & Service Pack: winxp pro v5.1 (sp2)
Graphics Card and Driver version: Nvidia Quadro fx540, 9.1.3.6
Amount of installed RAM: 3GB
Virtual Memory settings: APPS, total paging = 1024mb
CPU Type & Speed: intel pent 4 / cpu 3.00GHz

 

[Updraft]

dsgnr1,

Don't give up so quickly. A few words of encouragement are in order. . .

Toolbox is a terrific tool if it is properly setup and used. Your VAR should be able to give you more specific setup instructions, but here are a few points:
1. Setup TB on your network. There should be enough info in the SWX/TB Help or talk to the VAR.
2. Make sure that everyone's installation of SWX is pointing to this network location. We have setup one computer to be the "template" with all the screen, menu, and other settings including file locations. We then use the Copy Settings Wizard to save these settings (we actually save them in a network directory for this and other SWX stuff) and then run this file on the other computers to make sure all are pointing to the same TB, file templates, etc.
3. We learned how to make a copy of the TB database to our company standard and then invested some time in setting it up with only our fasteners and their part numbers and descriptions. Now when we insert a fastener we select our TB and then can select the fastener with a choice to pick from a list by part number or by description. SWEET! This TB only has in it what we have in our system so we do not have an overwhelmingly long list to search through.
4. When we need a fastener that is not in our list we simply access the standard TB to pull in that fastener to verify within SWX that it is the correct size. Then we will edit our company database to add the new fastener with its own part number. It is a simple matter then to change the other fastener to this company-specific version.

Making a separate file of all the fasteners is a kludge workaround. You will spend less time and have more more flexibility if you setup TB as it is intended to be.

- - -Updraft

 

[Waidesworld]

"Making a separate file of all the fasteners is a kludge workaround. You will spend less time and have more more flexibility if you setup TB as it is intended to be."

I agree with you but in reality we have about 50 max. fasteners that we use on a regular basis. It was quicker to extract these than to pare down the list.

drawn to design, designed to draw

 

[rgrayclamps]

Hi, dsgnr1:

Can you duplicate your problem if you start a fresh session of SW and open a new assembly document?

Best regards,

Alex

 

[dsgnr1]

Alex,
You are so right. re-booted, started a new session of SW and started a new assembly. Plopped the same piece of hdwr in that I was having trouble with and !viola! It works properly that way. What would be the culprit if you had to guess? The double install?

thanks again,
Jim

¿)
Version of SolidWorks: 2009
SolidWorks Sercive Pack:sp3
Operating System & Service Pack: winxp pro v5.1 (sp2)
Graphics Card and Driver version: Nvidia Quadro fx540, 9.1.3.6
Amount of installed RAM: 3GB
Virtual Memory settings: APPS, total paging = 1024mb
CPU Type & Speed: intel pent 4 / cpu 3.00GHz

 

[rgrayclamps]

Hi, dsgnr1:

The assembly document you are working on has a pointer to a different toolbox item loaded in my RAM. Models in RAM has first priority in SW reference. Two items with same name are not allowed to coexist in SW. Your SW thinks the toolbox item you are trying to insert is already loaded, which is true, and thus asking you to open it.

You need to examine your assembly carefully and get rid of those references, save it. Then restart your SW and open it again, you will be fine.

If you do not restart your SW, you may still have the same issue as SW is notorious not to release (dump) data in RAM memory upon closing a document.

Good luck!

Alex

 

[macduff]

Waidesworld,
We do the same thing as copying and renaming parts. I like breaking all ties with the SW TB parts, databases and all.

Colin Fitzpatrick (aka Macduff)
Mechanical Designer
Solidworks 2009 SP 4.1
Dell 490 XP Pro SP 2
Xeon CPU 3.00 GHz 3.00 GB of RAM
nVida Quadro FX 3450 512 MB
3D Connexion-SpaceExplorer

 

[dsgnr1]

ANOTHER STAR FOR RGRAY...
Removing the double toolbox problem fixed it. I tested this today and low and behold, no more "panheadcross is already opened. Do you want to view..."
AND:
as a bonus, the toolbox works properly now...no more jumping to extents and ending the screw drop function.

Such clear and concise instruction as well.

=)
thanks Alex!

¿)
Version of SolidWorks: 2009
SolidWorks Sercive Pack:sp3
Operating System & Service Pack: winxp pro v5.1 (sp2)
Graphics Card and Driver version: Nvidia Quadro fx540, 9.1.3.6
Amount of installed RAM: 3GB
Virtual Memory settings: APPS, total paging = 1024mb
CPU Type & Speed: intel pent 4 / cpu 3.00GHz