Tool Box 1

[Kartbuff]

Hello all...
Im running Sworks 2004 SP0.

Issue:

Two people are working on one common assembly. I finish some work on the assembly, add a few nuts and bolts via the toolbox browser, then I pass the assembly over to my partner so he can do some of his work to the assembly. He opens the assembly and all the hardware (nuts & bolts) have gone SUPERSIZED. Right click the bolt and edit toolbox definition, and the proper size bolt is listed but shows up 10x larger then actual. (ex 1/4-28 looks like 3")

Two different computers, both WinXP, both Sworks 2004 SP0

We do have a mix of metric and english hardware in the assembly. Will that matter??


Anyone know why the hardware is not being loaded properly?
or a possible fix.



Thanks alot....



Travis.C

Mech-Eng

 

[manxJim]

The problem is when you take something from the toolbox it SW makes a copy of the part in your toolbox directory in a folder called copied parts. This folder is on your hard drive witch is why your partner can see it so SW uses its default setting e.g. big nuts
You need to copy the tool box and copied parts folder to your network then set your toolbox browser to look at the new location
It’s a long time since I set one up so check the help for more information

 

[DesignSmith]

Kartbuff,

Your symptoms would also indicate 2 separate Toolbox installations, operating in parallel and not synchronized, rather than 1 shared installation with the data on a central location.
Compare the \Toolbox.ini file on both machines, it needs to match and needs to be pointing to a common mapped drive.
You can copy the corect file from machine to other as needed, or edit it with WordPad.
Full instructions for a Shared Toolbox Installation, are on-line in the subscription support area, or available from a VAR.

A slightly more remote possibility is a corrupt Visual-Basic installation on the second machine. In that case no hardware created on that machine will size properly and it will corrupt your good hardware as well. A quick check is to make a simple Length = 2*Diameter part equation. If that equation will not reset the dimension properly or evaluate properly, the VB on that machine is broken. A reinstall of SolidWorks or MS Office will fix a bad VB.
Once the VB is repaired, a manual rebuild on any mis-sized hardware configurations will fix them.



DesignSmith

http://www.DesignSmith-Services.com

 

[SBaugh]

Also check out the Guide on Setting Toolbox up in a multi-user Environment at the SW website.

http://www.solidworks.com/pages/services/subscription/ServicePacks.html?PID=252

Regards,

Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376

 

[oharag]

Okay, here are a couple questions for you!

In the past I worked at an organization that had individual installations of toolbox on everyone's computer. We would check files up into PDMWorks without Toolbox parts. Everything worked well. But, we would get the occasional substitute large HW in an assembly someone else created. I also experienced this when I burned files onto a CD-Rom and took it to my VAR. All the HW came in huge. Here's some comments/questions:

- Why the heck does Toolbox act this way?

It would seem everyone has the same Toolbox from Solidworks. Sure Toolbox is updated, and maybe a few fasteners are added or updated, but it would seem everything inside Toolbox would remain the same!!!!!! If you insert a Toolbox part inside an assembly, and then share that assembly with others (either through internal email, PDMWorks or external) Toolbox should be able to figure out which fastener was used, and how to rebuild that fastener. Sure, if it's a custom fastener than it would be appropriate for Toolbox to fail, but common fasteners should work ALLLLL the time.

We were told to go to a central network version of Toolbox, and this would solve the problem. The problem I encountered with past upgrades of Toolbox was that you had to go to each users computer to install the update. It would then ask for a location of Toolbox Part folder. We would do this ten times! I believe this has changed with newer updates of SolidWorks with Toolbox being part of the Solidworks service pack updates. Here's a couple of comments/questions:

- Why wouldn't Solidworks break apart the updates of the Toolbox plugin on each local computer and the Toolbox Parts Folder itself? Update each computer with a smaller updater, and then update the Toolbox Parts Folder separately.

- Is it possible to update the Toolbox Parts folder once, and skip the updating of this Folder for everyone else's update? The goal is to update the Toolbox ddl on the local computer.

I was told that during an update of Toolbox even though it asks for a location of Toolbox Parts, which had already been updated, the installer skips over updating the Toolbox Part folder. It doesn't seem like this is the case by watching the installer. It seems to reinstall the update over, over and over again!!!!

Of course I believe you need to perform the update of the Toolbox Parts Folder on everyone's computer because it updates the pointer to the Toolbox Parts Folder on everyone's computer. I believe we've figured out how to perform this update once, and then copy the Toolbox.ini file to everyone's computer. BUT!!!!! You still need to perform the update, and it asks for a Toolbox folder, yada yada yada.

- WHY WOULDN'T THIS BE MUCH SIMPLIER?????? Why can't I point to the Toolbox Parts Folder using System Options inside Solidworks? Why does it have to be hidden inside an obscure file located somewhere called Toolbox.ini?

Okay, now the most recent weird behavior!!!!!

Knowing all the problems with having individual installations of Toolbox Part Folders I made it a point to set everyone up using one Network installation of Toolbox Parts Folder. Everything seemed to work. We deleted the local Toolbox Parts Folder for everyone. There was a gentleman that created an assembly using Toolbox Parts from a local install. I read the installation notes from Solidworks. In the notes there is a section entitled "To automatically have the SolidWorks software to search for external references:" I followed this section. We performed the changes to the system options as recommended. When we opened the assembly everything seemed to work as expected. We checked this assembly up to PDMWorks (I'll get back to this later).

We've recently received an assembly from an outside contractor. He provided the toolbox part files along with the assembly. Someone copied the files over to his hard drive. He opened the assembly on his computer fine. When he checked the file up to PDMWorks (without Toolbox Parts) everything worked. The problem arose when someone else tried dling this assembly onto their computer. The Toolbox Parts are not rebuilt. We get an error message that the following Toolbox Part cannot be found would you like to search for it? I still have the "Search for external references" checked on everyone's computers. Everyone is pointing to a central Toolbox Parts Folder. Searching for a specific Toolbox Part by browsing to the Folder is a pain in the neck. And if you select the wrong fastener you have to redo the task!

- Why doesn't this whole Toolbox thing work flawlessly??????? A Toolbox Part is a Toolbox Part!!!!!

It's a shame something as beautiful as Toolbox can be so flawed! Why is so hard for Solidworks to figure out where Toolbox Parts are located, and why doesn't it figure out how to rebuild Toolbox Parts without user involvement??

Okay, so we decided to perform another test. I had someone create a very simple assembly from another company (we both had the same version of Solidworks and Toolbox installed). It had Smart fasteners inside the file. It also had Toolbox Browser Parts. I had them send the file to me via email. I copied just the top-level assembly and part file over to my computer (leaving behind the Toolbox Parts). I opened the top-level file, and was greeted with "Unable to locate Toolbox Part, would you like to browse?" I have the settings recommended by Solidworks in their install notes for searching for external references. And yet Solidworks cannot figure out how to rebuild Toolbox parts!!!!!!!!

Okay, one more test. I decided to create another very simple assembly. I used Smart fasteners and Toolbox Browser Parts. I checked this file up to PDMWorks without Toolbox parts. I had a colleague on the same network (same version of Solidworks pointing to a central location for Toolbox Part Folder) dl this file. Everything came down fine except for one screw and washer!!!!!!!!!!!!!!!!!!!!! This screw was part of a Smart Fastener config. It had a screw, washer and lockwasher. The only thing that displays is the lock washer. When this person goes to Solidworks Explorer and looks at the file locations for each part in the assembly it shows the 2 files that are missing are located on my Harddrive. The others are pointing to the Toolbox Folder on the Network. Is this because we both have "Search for external references" checked in our settings? I thought that Solidworks would always go the Network Folder for Toolbox first, and then search other locations next.

Now the files that had been supposedly checked up awhile back after having been redirected towards the Network drive come down with Toolbox Parts failed. What is wrong with this setup?

Sorry for the long post. There’s a lot of frustrating things going on with Toolbox. Again, you would think an integrated add-in inside Solidworks would work a whole lot easier and reliably than Toolbox today.

oharag

 

[DesignSmith]

Oharag,

Some of what you are seeing when you bring an assembly outside of your network, is due to the SolidWorks automatic file references finding. When you open an assembly, it looks for the parts in the original folders first, then the current folder, then all the way down your file search paths.
On your VARs machine, it finds the same file name, but with different configurations activated, and references that file into the assembly.
To change that behavior, goto Tools Options, and set your External References and File Locations settings such that part files are found in the preferred project folder first. Then simply close and reopen your assembly.

Another part of why each Toolbox installation is so unique, is that it only installs the 1000 basic part files, and the database in about 400Mb of disk space. It then provides the more than 5 million items through the power of dynamically creating configurations on the fly. Rather than installing 10s of Gigabytes of parts to your computer, it automatically generates only the sizes and lengths you actually use.
Not only does that technique make your installation smaller, it also allows for changing the size and length of items while they remain mated in your assembly, without the need to delete parts and reinsert them.

Although you can configure Toolbox and turn the Copy Parts option on, to always create new parts rather than new configurations. You give up SmartFasteners, and the edit in place capability in exchange for the easier assembly portability. Not to mention that the configuration approach reduces assembly storage for the hardware to 1/2 or 1/5 of what it would be otherwise. The individual part file sizes are larger, but fewer of them are needed to supply the same range of items and sizes in large assemblies.

If you have switched from more than a couple independent Toolbox installations to a shared installation and are still have sizing problems, it is very likely there are duplicate Toolbox directories floating about your network.
Toolbox 2001 Plus and newer does allow for synchronization with PDMWorks, but the proper installation and setup of products is not trivial.
For more than 6 users, it may well be worth getting a VAR AE involved, bringing in an independent CSWP, or assigning someone the temporary task of library administrator.
During the process of properly configuring and rolling out the library, they can fine tune the standards and sizes that you want available in your firm, thus helping to keep your designers more consistent with the hardware they use.



DesignSmith

http://www.DesignSmith-Services.com

 

[SBaugh]

It would seem everyone has the same Toolbox from Solidworks. Sure Toolbox is updated, and maybe a few fasteners are added or updated, but it would seem everything inside Toolbox would remain the same!!!!!! If you insert a Toolbox part inside an assembly, and then share that assembly with others (either through internal email, PDMWorks or external) Toolbox should be able to figure out which fastener was used, and how to rebuild that fastener. Sure, if it's a custom fastener than it would be appropriate for Toolbox to fail, but common fasteners should work ALLLLL the time.

That's because as you add your fastener to your assembly. Then and only then is a configuration ADDED to that TB part and since it is found on your local HDD it will not be avaialble to others who open that file. You ask "Why's that?" I'm sure. If you were to look at the path that SW has saved for the TB part you will find that is looking a "C:\Program Files\Common Files\Solidworks Data\Browser\Ansi Inch\ etc..." Well if you colleague opens up that same assembly. Guess what SW is going to follow that same path. It's going to find the same part but it's not going to find the same configuration.

- Why wouldn't Solidworks break apart the updates of the Toolbox plugin on each local computer and the Toolbox Parts Folder itself? Update each computer with a smaller updater, and then update the Toolbox Parts Folder separately.

For one I'm sure it's because of the WI installer. Two - I'm sure customers requested this to count down on the amount of installs. I'm sure the IT Dept is happy with this.

- Is it possible to update the Toolbox Parts folder once, and skip the updating of this Folder for everyone else's update? The goal is to update the Toolbox ddl on the local computer.

I'm sure it might look like it's replacing those files (This is if your using a Network install, if not then you will need to run this for each computer) You have to remember SW is trying to write one program to do 2 different things. One it has to install for Network users and two it has to install for Standalone TB seat holders.

- WHY WOULDN'T THIS BE MUCH SIMPLIER?????? Why can't I point to the Toolbox Parts Folder using System Options inside Solidworks? Why does it have to be hidden inside an obscure file located somewhere called Toolbox.ini?

SW bought up Cimlogic which was the company that came up with this. I'm sure it might just come down to the fact it's easier and cuts cost by keeping it like this. By putting in the System Option File locations would cost more time and money. Some of you here complain about how they need to spend more time on stability. Well if that's the case then this wouldn't fall into that category.

- We've recently received an assembly from an outside contractor. He provided the toolbox part files along with the assembly. Someone copied the files over to his hard drive. He opened the assembly on his computer fine. When he checked the file up to PDMWorks (without Toolbox Parts) everything worked. The problem arose when someone else tried dling this assembly onto their computer. The Toolbox Parts are not rebuilt. We get an error message that the following Toolbox Part cannot be found would you like to search for it? I still have the "Search for external references" checked on everyone's computers. Everyone is pointing to a central Toolbox Parts Folder. Searching for a specific Toolbox Part by browsing to the Folder is a pain in the neck. And if you select the wrong fastener you have to redo the task!

- Why doesn't this whole Toolbox thing work flawlessly??????? A Toolbox Part is a Toolbox Part!!!!!

You need to search up a KBA at the SW website on the "Reference Document Search Routine" That might help explain to you how SW looks of reference files.

Okay, so we decided to perform another test. I had someone create a very simple assembly from another company (we both had the same version of Solidworks and Toolbox installed). It had Smart fasteners inside the file. It also had Toolbox Browser Parts. I had them send the file to me via email. I copied just the top-level assembly and part file over to my computer (leaving behind the Toolbox Parts). I opened the top-level file, and was greeted with "Unable to locate Toolbox Part, would you like to browse?" I have the settings recommended by Solidworks in their install notes for searching for external references. And yet Solidworks cannot figure out how to rebuild Toolbox parts!!!!!!!!

That's because the Toolbox parts don't have the same configuration as the parts that were saved in the assembly. It sounds like to me you want SW TB to rebuild each bolt in your DB to match the assembly file. That's not possible. It probably won't be either. If that was the case then we would have a problem because if TB parts couold do it then that would most likely mean SW parts could do it. I can't imagine the problems that would occur with this in place.

The others are pointing to the Toolbox Folder on the Network. Is this because we both have "Search for external references" checked in our settings? I thought that Solidworks would always go the Network Folder for Toolbox first, and then search other locations next.

You need to look up that KBA I listed above.




Solidworks Highly doesn't recommend the use and checking in of Toolbox parts with PDMworks. They did provide a very useful way of using TB over a multi-user environment (Finally). I have several users, using this tool in the same type of environment and I never have get any compliants from them on this. TB is not perfect or flawless, but it's a lot better than it has been. If you have some suggestions, why don't you instead of complaining, try entering in some ER (Enhancement Requests). You have some good ideas here and I think there are some that would agree with you. If you do place and ER in.

Regards,

Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376