Have you ever opened an assembly, and all the Toolbox components were huge? But last time you opened this assembly it was correct? Toolbox is the most popular of the Professional Add-ins, but it is also the one least understood.
Q: So what is the deal with the HUGE Toolbox component sizes? Why would an assembly open with hardware that looks like it belongs on a tractor, yet we are designing micro motors…
A: SolidWorks acquired CIMLOGIC, the programmers of Toolbox/SE, on Nov. 27, 2000. Just some toolbox trivia so it has been around for a little while in SolidWorks. The reason for the different toolbox sizes is simply having different toolbox databases being referenced.
The toolbox is a collection of hardware that ‘thankfully’ we don’t have to model. But when you consider what that actually means, it means that this database could contain every variation of size for each fastener. For example a Socket Head Cap Screw from the Ansi Inch standard alone has 32,988 possible configurations according to SolidWorks Toolbox 2009 (of which does not include material verations that the use could configure into the toolbox database easily doubling this amount).
Now the problems of organizing and file storage should become obvious. As this toolbox database and amount of associated SolidWorks components/configurations would be huge. It is impractical to expect users to install over 10+ gigabytes of information for each S0lidWorks workstation toolbox installation.
The toolbox generates a size for a given fastener only after a users manual input asks for it. As the new sizes are requested then new configurations/files are created. However if the same assembly is opened on another system with it’s own Toolbox database, then the default configuration of the fasteners will be used if the referenced size is missing. The default size is the ‘large’ fasteners, so as to make it obvious that the toolbox components needs to be corrected.
The solution: Always use a ‘Shared’ Toolbox from the network. This will ALWAYS WORK!! So long as you generate your hardware from the shared toolbox, then the shared database is updated.
SolidWorks solution: Software enhancements were added to assemblies in version 2007 to correct this issue. This enhancement basically stores toolbox information about the sizes of hardware it references with that assembly file. Now when the assembly in a new toolbox database environment, Toolbox will offer to create the missing referenced fastener sizes(provided the toolbox is added in at the time of opening the file). But here is the catch, this only works in SolidWorks 2007 or newer generated assembly files…
The above solutions work for a company that had started with a shared toolbox in the beginning, or started working with toolbox around the SolidWorks 2007 release.
Work around: So this is for the rest of us who have been using SolidWorks long before the 2007 release, and yet still need to send out assemblies to be reviewed by other SolidWorks users. The recommended solution to generate a 2007 or newer assembly with all the toolbox components and sizes that you use frequently. Thus when you need to work with a new toolbox, you can open this assembly first. Your hardware assembly will generate all the sizes that you need. This is a great tip for those of you working with other design houses. You can send them this hardware assembly first, so they can educate there toolbox to accomidate your assemblies.
Legacy files: Another potential solution is to generate a 2007 or newer assembly, and insert your old assembly. Now dissolved your sub-assembly of that old assembly (*Please note that this can be destructive to any assembly using in-context design techniques, and will eliminate any exploded views that you have. It is not recommended for assemblies with configurations unless the same configurations are added to the new assembly and matched via the sub assembly BEFORE you dissolve it). Now when you save this, your new assembly will have the toolbox data necessary to recreate fasteners on a new system.
These solutions only addresses the physical sizes of the models for the hardware in the assembly. The main reason for a shared toolbox includes addressing customer specified part numbers and descriptions. As this information is NOT included in the assembly file information.
Additionally any non-default configuration names, added for example, to accommodate material variations as file properties for toolbox fasteners. These non-default configuration names will result in the warning dialog that the specified configuration cannot be found. The last saved configuration will be used instead.
Finally custom toolbox parts, that is parts you placed into the toolbox, will not be ‘generated’ on another system.
Conclusion: A shared toolbox is always recommended, please see the install guides here for more information. For the mapping of Toolbox database, it is Tools/Options, HoleWizard/Toolbox, and browse to the shared database.
