What is SolidWorks Toolbox?

This is part 1 in a series just on Toolbox. It has started from the series on CAD Admin. Toolbox is not a topic that you can talk about in a single long blog post, there is just too much there, if you’re gonna do the topic justice.

Toolbox may not be exactly what you think it is. The image to the left shows how SolidWorks describes Toolbox in their Product Matrix. They call it a “Standard Hardware Library”, and say that you have access to “pre-built SolidWorks models”. It may be picking nits, but strictly speaking, neither one of these statements is true.

When I think of a “library”, I think of a place where I can go to get something that is there, something that exists. Toolbox doesn’t really work that way. With Toolbox, you tell it the class of thing that you want, and it builds it for you. This may or may not be an important distinction for you.

Toolbox consists of 3 parts:

1. Toolbox application – software that “does stuff”
2. Library of blanks – SolidWorks parts used as templates, which contain all of the geometrical options available
3. Database – contains all of the dimensional and “metadata”  used in the finished parts

If you have a real library, all you have is #2. So having software and extra data in a database is extra, and should be better, shouldn’t it?

Yes, and no. It is better than just a library because of things like Smart Fasteners. SF enables you to automatically place the correct sized hardware into holes automatically. The problem is that it only really works that way in special situations. So you could say that it helps some of the time, and just gives you something to undo some of the time.

So in a nutshell, here is how SolidWorks Toolbox works:

1. By default Toolbox installs as a single user installation, where the library is local. There are many options during install in 2009, and I’ll talk about those in a futurearticle. Libraries can be shared or local.
2. By default the Toolbox database installs locally, but it can also be placed on a network for a shared install. The database is called SWBrowser.mdb, is typically located in a folder called C:/SolidWorks Data/lang/English, and for SW09 sp3.0 is 87.876 MB. You can browse and edit the file using Microsoft Access.
3. Toolbox is an add-in, so you have to activate it using the Tools, Add-ins menu. It is really 2 add-ins, SolidWorks Toolbox and SolidWorks Toolbox Browser. What I am talking about here is mostly the Browser. This is the user’s first clue that Toolbox is not just a library, it’s also an application, software.
4. Toolbox is used by drag and dropping Items from the Task Pane into the Solidworks graphics window. (There are also other ways to get parts into an assembly.) But before you do that, this is what you are confronted with, shown in the image to the right: a list of standards. Yes, but you can trim down that list of standards so it isn’t nearly as irrelevant. True, you can, but why hasn’t it been done? This is the way it was installed, even though during the install you specified ANSI standard and Inch units.So you have to configure the standards a little. You might even find after using it for a while that what you really need is a custom standard. Fortunately, it’s easy to do, but the hard part is first figuring out that it needs to be done at all, and then where you go to do it.

   It turns out that you have to go to Toolbox, Configure Toolbox, Select Your Hardware. From there you should just unselect any standards from the list that you don’t want to use. Be aware that when you open the Configure Toolbox dialog, it may take some time, because SolidWorks is opening up that 88 MB database file in the background. If you have a shared install, it may take even longer because the database has to be opened over the network.

5.  After you get the standards set up, you drag and drop the type of screw onto the edge of a hole. Toolbox should orient it correctly, but if it doesn’t you can always press the Tab key to flip it 180 degrees.At this point, Toolbox asks you to choose a size and gives you some other options. If your Toolbox is a fresh unused installation, the part that Toolbox is using has only a single size, which is most often the largest size in the library. When you select a size from the interface, Toolbox selects the dimensions for that size, and creates a new configuration in the fastener.

   But hold it. What if this is a shared installation? Or what if I get an existing assembly with my new Toolbox installation?

   Well,  in those cases you should have known something prior to getting put into that situation. Again, most users find all of this out by accident, and usually after they have lost a lot of design data in assembly files. There are answers to each of these questions, but the fact is that many users don’t even know that the questions exist until it is too late.

As you get deeper and deeper into Toolbox, you come across many scenarios that may not be ideal for you. In almost all of these situations SolidWorks has provided for a way to resolve the issue in some fashion. The problem is knowing there is a solution, because solutions are not always obvious, and in many cases knowing there’s the potential for a problem, again because the need for a solution is sometimes not aparent until it is too late.

The truth is that the default installation settings work well for a stand alone user who does not share data with other Toolbox users. But the default settings can be disastrous for other types of use scenarios.

This Toolbox subtopic of the CAD Admin series will continue in a future post.