Toolbox frustrating issue

The only way out is to dump Toolbox and create your own library.  For years I used my own library, then SW came out with the toolbox and it was the greatest thing since sliced bread, I used it for a year, had tons of models with a lot of fasteners. All was working awesome till.... we upgraded to the next version, there was a huge bug in Toolbox and I would open a model and all my fasteners were way oversized, a 1/4" bolt would turn into a 1" bolt and it affected everything I had worked on for a year....... never again...

Assuming you are not using EPDM and an EPDM controlled toolbox?  I have always seen this behavior when toolbox is installed locally, but never seen it when installed on and controlled by EPDM.  I've never tried sharing it off a netwrok drive without EPDM control....

If you install it on a mapped drive, and make sure all the workstations have the same mapping and all point at that location for the toolbox, will that solve your issue?  May be worth a try, if you haven't already. 

Hi! I prefer to save every Toolbox part that I use for myself. After it, you need to run sldsetdocprop.exe (Program Files\SOLIDWORKS Corp\SOLIDWORKS\Toolbox\data utilities\) to change property state. This way it becomes independent and I presume that is prevents you from accidents.

Hi Alex,

1. Are all of the users pointing to a single Toolbox installation on a network folder?  This is the best method to use Toolbox with multiple users so that all have the same data to work from.  This way data doesn't change depending on which user added hardware to an assembly.  Just like any file, if you have multiple files with the same name on different computers that users are adding, you will get varying information in the assembly tree and BOM.
2. If working from a network location, have you assigned an admin for Toolbox and created a password to prevent others from changing the settings and data?  This safeguards the integrity and consistency of your data.
3. If you used to see the name of the piece of hardware in the model tree, you may have changed one of two things:
   1. You may have changed the setting on page 3 of Toolbox Settings to control the Display options (see first image below, from left to right: this is where the option can be found, display of the Description property in the model tree).  This will override the display of the filename in the tree to a property of your choosing.  Once this setting is saved, it applies for all newly added or edited hardware.
   2. You may have turned the Show Component Configuration Names option off in your model tree to display (see second image, from left to right: option is on and configuration name is shown in the tree, this is where the option can be found, option is off and configuration name is not shown in the tree).  This setting can be set in your default assembly template and will apply to all assemblies created thereafter.  Existing assemblies need to have this option set for each one independently.  You could likely write a macro to apply this setting to legacy assemblies if needed.

I hope this helps,

Jody

The way I do it is open the toolbox part in Solidworks, and then do a save as and give it an actual name.  This way you have the toolbox part, but it is no longer tied to the toolbox.

I even made configurations for multiple lengths of bolts / screws in a single file, so you can change the length of the bolt / screw in the assembly by selecting it from the drop down box (See Pic).