SolidWorks Toolbox Bible

This is a chapter I wrote for the SolidWorks Administration Bible about 10 years ago. It is still mostly valid today. There was a discussion on the SolidWorks forum that led me to post this. I think folks have not carried the torch lit a decade ago by those of us who researched and understood most of this topic.

This was about 26 pages in the original, and slightly edited here. Worth reading if you wrangle Toolbox on a regular basis.

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Toolbox

If you as a SolidWorks Administrator are new to SolidWorks Toolbox,
you need to read this chapter. In fact, I recommend all potential
SolidWorks customers read this chapter before buying the SolidWorks
software. Toolbox is an add-in for automating tasks related to inserting and
managing commonly used library type parts; and you will get the most out
of it if you understand and configure its options early on.

The promise is automation, and the implication is that it works automatically
right out of the box. However, the default installation is very far from the
configuration in which it actually works best. Both SolidWorks and Toolbox
are very complex. This chapter guides you through all of the options and
setup parameters available with Toolbox.

Before I discuss how best to implement Toolbox, I cover exactly what
Toolbox is, how it works, and why it is as complex as it is. Only then will
you be ready to work through various scenarios to see which Toolbox configuration works best for you.

If you only look at Toolbox’s individual options, you may never understand
everything it does because you are not aware of the big picture. As
Administrator, you need to know the capabilities and the limitations of the
tool, as well as understand how flexible it is and where its weaknesses lie.
All this goes much deeper than the simple button-push tutorials you will get
from most other sources for Toolbox. Understanding the larger picture may
make you more tolerant of foibles in the software because you know the payoff
can be great. Seeing the overall vision for the software may make you
rethink the common wisdom that you should not allow your tools to determine
your workflow.

In the past, many people (including myself) have looked at Toolbox as an unmitigated disaster of implementation. Those days appear to be largely behind us, and if you look at Toolbox’s functionality in detail and try to understand why it works the way it does, you will see that if nothing else, the vision driving the creators of the software is very compelling.

Understanding Toolbox
SolidWorks calls Toolbox a library. A library, in CAD terms, is a central place where you can go to get parts that might be shared between multiple products. A more general definition of a library might be that a library is a place you go to get things that exist, as opposed to something like a custom order catalog, where you go to get things that currently don’t exist, but will be made for you. Another aspect of a library is that it is relatively static. A library has many items from the start. You
can add more items to the library, but if you buy a library, you expect it to start out well stocked. Again, Toolbox differs. It doesn’t start out with many items. It starts out with one of every item, but there may be thousands of many items.

It sounds like an academic distinction; can it be important? In the end, you still get your part, right. Well, yes and no. For example, in CAD you share your parts, so that many users can use the same part over and over again. On the other hand, you may send your assembly to someone else, and they are expected to have the same parts in their library that you have in yours. The main problem is the people who need to know all this information are new customers, and new customers are the last ones to find out that this information exists and realize they need it
desperately — before they proceed.

Am I dramatizing this? A little, maybe. In the past, it was certainly true that improper Toolbox implementation could result in significant data loss. That is not true so much with versions that are more recent. The main risk now is that you don’t know all of the implementation options, or that functionality such as Smart Fasteners does not live up to its billing.

By any measure, this is a lot of functionality in a single SolidWorks add-in, and a lot of functionality to show you how to administer in a single chapter. While this book does not cover how to use the features, it does cover how to administer the functionality, including setup and settings. For more detailed information on how to use the various functions in Toolbox, check out the SolidWorks 2009 Bible (Wiley, 2009), or current version.

Understanding how a default Toolbox installation works
Toolbox is not a library. Rather it is a “configurator.” People who work at SolidWorks don’t agree with this assessment, but I’m judging it by what it does. A configurator is an application that custom builds a product for you based on your answers to a set of questions. For example, you might go onto the Web site of an automobile manufacturer and specify that you want the LX model in blue with the upsized engine and MP3 player input. Then this configuration appears
on the screen. That’s essentially what SolidWorks Toolbox does.

SolidWorks Toolbox has three components: the database, library parts, and program that automate it all. Toolbox takes the input from the user interface and compares it with the database, then uses numbers it retrieves from the database to add a configuration to the part in the library. The default part in the library is usually the biggest or smallest size available from the database. All the numbers
for all the sizes are available in the database. In this way, every time you create another size fastener, Toolbox adds a configuration to the part. You can set it up to work differently, but this is how it works by default. This process is shown in Figure 10.1.

The basic Toolbox process shows schematically how Toolbox works.
Input size and options through user interface Toolbox gets data from database
Database feeds dimensions to SolidWorks SolidWorks creates a part configuration
I’m sure the reason SolidWorks installs library parts with only a single size is to save space and time during the installation. If you had to create all the sizes of all the fasteners, it would take a great deal of time and a lot of space. Is that a bad thing? This is a question that you will have to answer for yourself. The Toolbox Configuration utility enables you to create all the sizes for a given Toolbox part, whether you are using configurations or individual parts.

The Toolbox default install
When you install Toolbox, and just accept all the defaults, it installs a full database, an empty library, and a set of program files, all on a single machine. Toolbox with all the default settings is really only meant to be run on a single machine where the user does not share assemblies with other Toolbox users. Ironically, things work okay if assemblies are shared with non-Toolbox users. I’ll cover the database first.

The Toolbox database
The Toolbox database is named SWBrowser.mdb, and for SolidWorks 2009 and 2010 is about 90MB in size; by default, is located at C:\SolidWorks Data\lang\English\. As you start using Toolbox and making hardware parts, the size of the database may grow significantly, particularly if you create a “user defined standard,” which I discuss later in this chapter.

The end user has no need to do anything in the Toolbox database, and even an Administrator shouldn’t take on database customization unless she is well acquainted with Microsoft databases. The size of the database (about 90MB in default arrangement) can be of significant concern for some situations, such as when sharing a database between users across a network, or even just
opening it on machines with low resources.

As with every other kind of data, it is important to back up your Toolbox database if you make any changes to it. Fortunately, if you do make a mistake, it is always easy to get a copy of a default database back by simply performing a default install of SolidWorks. You should keep a full version of the default database available in an archive, and if you customize Toolbox, you should keep a
copy of a modified version. Backing up Toolbox data is simple: it requires only a single top-level folder to be copied, the \SolidWorks Data\ folder. The backup is as simple as copying the folder to another location, and the restore is as simple as overwriting the folder and contents. (It is recommended to rename the old folder before restoring a copy of the folder.)

One thing to remember that can complicate the backup Toolbox database issue is that each version of SolidWorks uses an identifiably different version of the database, and the database version might be tied to versions of the library. If your company uses multiple versions of SolidWorks, maintaining versions of Toolbox can be a significant challenge.

The part library
The Toolbox part library is located in the Browser folder under the SolidWorks Data folder. When the library is initially installed, each part has a single default configuration sized at either the high or the low end of the size range (biggest or smallest available size). These parts have features, some of which are suppressed depending on settings. All parts use Mate References. Mate References are
stored faces or edges that are used as default mating entities when inserting Toolbox parts. For more information on how to create or use Mate References in SolidWorks, refer to the SolidWorks 2009 Bible (Wiley, 2009).

Program files
The program files for Toolbox are kept in the \Program Files\SolidWorks\Toolbox folder, as a set of *.dll files. You will not have any need to access or edit these. These files are updated with new major releases and service packs.

Managing Toolbox data
Managing SolidWorks data is a big issue that you have to understand as a SolidWorks Administrator. When you add Toolbox to the mix, you might expect that SolidWorks Corp has already thought of something clever for managing Toolbox data, but, in that respect, you might be disappointed. In fact,
the major conceptual flaw in Toolbox is in how it handles data management issues.

Underlying basic flaw in Toolbox
If there is a basic underlying rule for SolidWorks data management, it is that you need to ensure unique filenames for all documents, and its corollary that you should not have multiple files with the same name accessible by the software, especially if those files with the same names have different content. The designers of the Toolbox software have allowed situations when the rules are very
easy to be violated. In truth, it doesn’t appear that they considered the file management issues inherent in a configurator application until it was too late. Even now, with all the small fixes they have implemented for all sorts of various small issues, and not so small issues, the file management problem is not one they have addressed with conviction. A real answer to the file management
problem is a static library. SolidWorks is a very progressive company, and may see this as unnecessarily timid. Given the problems with the dynamic library, I believe the static library to be prudent.

Beyond the gross file management issue, if you want to include custom property information with your Toolbox parts, and make sure that data is propagated to copies, you may run into difficulties making sure that happens. The model of a static library of parts that you can count on is very difficult to achieve and maintain in Toolbox.

Carrying it all a step further, say you want to add material classifications or even something like point type (such as cup point, nylon point, dog, half-dog, and so on) to screws, or flags for selftapping threads or nylock thread locker. You can add these types of things, but doing so, and maintaining that information between releases of SolidWorks, can be time-consuming and difficult to figure out initially and troubleshoot.

You can work around the file management problems, and the custom property problems and the material/finish/point/thread treatment classifications, but each one of those issues requires a separate solution, and each has limitations, some of which you may need to discover and solve for yourself. Toolbox is certainly capable, and full of functionality, but the way that it is all put together, you have to wonder if the effort to get the solution is worth it.

Configuring a multi-user installation
Many SolidWorks installations consist of multiple users. When multiple users have to work together, they need to avoid the default single-user Toolbox installation. Figure 10.2 shows two situations: one with multiple users using the default single-user Toolbox and another with multiple users sharing a Toolbox installation.

Multiple users with individual and shared Toolbox installations

Another issue that comes up with this scenario is the speed problem of opening the database across the network, beyond the overhead of the assembly and parts. To counter this, you can put the database local to each user, but you have to make sure that the two users are using the same Toolbox settings before copying the database.

Therefore, that solves some of the problems, but problems with write access on the library parts remain. If you make the libraries local, you’re back to the same situation that you started with. The available sizes in one library do not match the available sizes in the other library, so sharing assemblies that might call for missing configurations between the users is not possible.

The obvious solution here would be to fully populate one library, and copy it to both users. This is a great solution, but it can be time-consuming. However, it gives you the option to add custom properties before copying.

Combining libraries
New users often simply install the software trusting it will work without doing much research beforehand. If you do this when Toolbox is involved, and you have multiple users, you will wind up with each user installed as an individual user without shared Toolboxes. If the users use Toolbox when it is installed this way, you will wind up with many individual libraries with different size configurations created in different parts.

Many times users ask if you can combine the configurations from one library with the configurations from another library. The stock answer to this question is no. SolidWorks does not offer a direct way to combine configurations between two different parts.

A method does exist for making this work, but it isn’t really intended for this purpose. If you have two parts with configurations and you want to combine the configurations into a single part, the only way I know of to do this is to use the Auto-create Design Table functionality to convert the existing configuration data into a design table, then export the design table and import it into the other part. This will re-create the configurations from the first part into the second part. It is not a very direct method, and if you have configurations from a large number of parts that you need to combine, it can be tedious, but the method works, and as the only method that works, it has advantages.

Administering Toolbox
Toolbox as an add-in requires almost as much of an administrator’s attention as the rest of the SolidWorks software combined to properly understand and implement. As an Administrator, Toolbox has plenty of things to keep you busy. The first thing to tackle is how to install Toolbox. I explain how to do it here, as well as how to make changes to existing installations and upgrade Toolbox.

Installing Toolbox
Toolbox is typically installed along with the rest of the SolidWorks software during a standard installation. During a SolidWorks 2010 Installation Manager installation, one of the options in the Summary section of the installation workflow is Toolbox Options. If you do not change the default settings, Toolbox defaults to C:\Solidworks Data\.

Cross-Ref
The standard SolidWorks installation procedure is detailed in Chapter 6. n
You can install Toolbox two ways:
l Local Toolbox. Located where the SolidWorks Data folder is on your local machine.
l Shared Toolbox. Located where the SolidWorks Data folder is on the network.

Each method has strengths and weaknesses, and neither is a silver bullet. If you want to create a local Toolbox, follow the default installation workflow.

Installing a shared Toolbox
If you want to install a shared Toolbox between several users, direct the initial installation Toolbox Options path (see Chapter 6) to your network drive. For subsequent installations, use the Use an existing Toolbox option.

After you have installed the folder to the network location, set the SolidWorks Data folder to Readonly.
You may need special user privileges on the server to accomplish this task.
1. Right-click the SolidWorks Data folder (displayed as SolidWorks Data 2010), as
shown in Figure 10.4, to open the SolidWorks Data 2010 Properties dialog box.
2. In the SolidWorks Data 2010 Properties dialog box, select the Read-only option.
3. Click Apply and then click OK.
The Confirm Attribute Changes dialog box appears.
4. Select the Apply changes to this folder, subfolder, and files option, and click OK.
The reason for setting the files and folders to Read-only is to prevent conflicts of file ownership if PDM software is not utilized. Toolbox will manage the write access it needs when the software creates
new configurations and wants to save them back to the file.

Creating a shared Toolbox from an existing installation
As soon as you install Toolbox and begin using it, making changes to the installation becomes more and more complex. Using Toolbox changes the library, so there is an important difference between a brand-new library and one that has been used even once. If you have an existing Toolbox that was installed locally, and you want to create a shared Toolbox installation from it, you have more work  to do.

You may want to create a composite Toolbox from several users who have already been using the software (because few people learn about the settings that they need to know before they do their first installation). You may have users who have created different parts, and, therefore, have different size configurations created in their default library parts. For this reason, if you try to open one user’s assembly with the Toolbox library from a different user, you will find that some  configurations are missing. Figure 10.5 shows the warning message you get if the assembly calls for a configuration that does not exist in your Toolbox library.

The functionality of Toolbox can only re-create a missing Toolbox size when the assembly was created in version 2007 or later. This does free you from worrying about potential data loss from sharing data with other Toolbox users, but if you choose to use the Copy Parts option (saves copies of parts instead of using configurations), the automatic configuration creation will not benefit you,
because it will never be needed. Configurations are a fantastic tool, but missing configurations in library parts does not improve the situation.

FIGURE 10.5
Warning message for a missing Toolbox configuration

Combining configurations from multiple parts
One of the difficulties in combining libraries is that there is no good way to do it. SolidWorks does not have an automatic way to combine the configurations of sets of parts into a single part containing all the combined configurations of both parts. The quickest way to combine configurations is:

1. Use the configured Toolbox part to auto-create a design table.
2. Auto-create design tables from each of the parts with configurations you want to combine.
3. Use the design tables to add configurations into one of the parts.

This method works, but it is not automatic, and if you have many different types of parts to combine or many users from which to combine data, it becomes tedious quickly. For more in-depth information on using design tables and auto-creation, check out the SolidWorks 2009 Bible (Wiley, 2009) or the current version.

Setting up the moved Toolbox
Follow these steps to make a shared Toolbox from an existing Toolbox:
1. Select the Toolbox library of the user who has created the most parts using
Toolbox, or use the steps described earlier to create new library parts using design tables.
2. Move or copy the \SolidWorks Data\ folder, including the newly combined files in the \SolidWorks Data\Browser\ folder, to the new network drive location.
3. Set the top-level \SolidWorks Data\ folder to Read-only, as described earlier in this chapter.
4. For each SolidWorks installation intended to use the shared Toolbox, choose
Tools ➪ Options ➪ Hole Wizard/Toolbox and set the folder to the network location of the \SolidWorks Data\ folder.

Note
It is preferable to use a UNC (uniform naming convention) path rather than a mapped drive letter because the UNC is more explicit, more consistent, and less vulnerable to change. An example would be \\servername\ AppData\SolidWorks Data\ rather than P:\AppData\SolidWorks Data\. Mapped drives can be mapped differently on different computers, but the UNC path to a specific network location is always specific as long as the server it refers to remains on the network. n

Upgrading Toolbox
If you have a stand-alone installation of SolidWorks and an individual Toolbox, upgrading Toolbox happens in the course of a regular SolidWorks upgrade. This is true whether you are upgrading between SolidWorks versions or just updating a service pack. SolidWorks may provide new executables (Toolbox programming), a new database, and new library parts. The executables should never be a problem, because neither you nor your users should need to edit the executables.
However, the database and the library files are different; you are expected to edit the parts at the very least. If you make changes to the database or library and then upgrade, SolidWorks may overwrite your changes in a way that is not recoverable.

Of course, you can use manual methods to deal with this problem, which include backing up your files or performing the upgrade and then overwriting the upgraded files, but even conceptually, this only works for service pack updates. The database could potentially be highly restructured between SolidWorks versions, and if SolidWorks recognizes that the database is an older version, it
kicks out an error message like the one shown in Figure 10.6.

FIGURE 10.6
An error message when the Toolbox database is older than the current SolidWorks version

Straight upgrades, where you simply upgrade one version of SolidWorks to another, are not recommended. If you want to upgrade from SolidWorks 2009 to 2010, for example, install 2010 as a separate version, leaving 2009 in place until you don’t need it anymore, at which point you can uninstall it. Keeping parallel installs of different major versions does not pose a risk to your computer
or SolidWorks installation. In fact, you can even run two different major versions, such as SolidWorks 2009 and 2010, at the same time.

Note
The one thing that is not allowed is to have parallel installations of the same SolidWorks version at different service packs. For example, SolidWorks 2010 SP 0 and SP 1 could not exist on the same computer at the same time.

Dealing with version incompatibility in Toolbox
Here is another conundrum you can run into with Toolbox. What happens when one person in your group upgrades SolidWorks versions? If this person upgrades the shared Toolbox along with SolidWorks, other Toolbox users will receive a version compatibility error, at least from the new parts in the library, if not also the database. If the person upgrading does not upgrade his Toolbox, he will receive his own version incompatibility error for the database, but the parts will not give him an error. If he adds a configuration to a part in the library, the part is saved in the new version, and then when users of the older version use that part, they will get the future version error. Upgrading and keeping both versions

Here’s how to deal with the version incompatibility issue in Toolbox. First, correct people who call this “backwards compatibility,” because that simply is not the case. It is, in fact, version incompatibility. Say you intend to upgrade from SolidWorks 2009 to 2010. You plan to have parallel installs, but you realize that if you simply install 2010 with Toolbox, your 2010 Toolbox will be a default
Toolbox, and you will be missing all the configurations and customization you added to Toolbox over the past year.

You also realize that you cannot just use the 2009 Toolbox because if SolidWorks 2010 updates any of the parts, SolidWorks 2009 will not be able to read them anymore. To have a functional 2009 and 2010 Toolbox, both functioning on the same computer without losing any of the work you did to the 2009 Toolbox, follow these steps:
1. Copy the \SolidWorks Data\ folder to a new location. You may notice that in some of the screen shots of my setup, I identify the version of the SolidWorks Data folder, such as SolidWorks 2010 Data or SolidWorks Data 2010. Copy and rename the folder with the included data.
2. When installing SolidWorks 2010, point the Toolbox Options (in the Summary of
the installation workflow) to the existing folder \SolidWorks Data 2010\.

This makes use of your old library with all its included parts, as well as the old database with any setup you have done. The install updates the database, but the parts are not updated until they are used, changed, and saved.

The one drawback to this process is that if you make any changes to the older Toolbox, they do not propagate to the newer Toolbox.

Configuring Toolbox
To get the most benefit from Toolbox, you must configure it. Default settings are intended for a single user who never shares files, and these settings do not work well in other situations. To begin to understand all the options you can control to make Toolbox as usable as possible for your organization, you must examine the Toolbox Configuration Wizard. As I mentioned earlier, Toolbox has a dazzling array of options when it comes to settings. This section of this chapter is meant to
help you make sense of everything, and understand what is critically important, what needs your attention, and which things are simply optional.

Starting Toolbox
To get started configuring Toolbox, first make sure Toolbox is turned on, and understand how to access it. Toolbox is located either in the pull-down menus or in the Library tab of the Task Pane to the right side of the SolidWorks window.

Toolbox is an add-in you must access through the Tools ➪ Add-ins menu.
To activate the Toolbox add-in, you can click the Add in now link or, to have more control over how Toolbox starts up, choose Tools ➪ Add-ins. In the Add-Ins dialog box, notice you have a selection of add-ins and two columns of boxes to select.

To have access to all the functionality of Toolbox, you need to activate both SolidWorks Toolbox and SolidWorks Toolbox Browser. The difference between these two is that the SolidWorks Toolbox adds the tools accessed through the Toolbox drop-down menu, shown in Figure 10.9. The SolidWorks
Toolbox Browser adds the more popular fastener creation tools found in the Task Pane.

The Toolbox drop-down menu offers access to calculators and other library-feature type tools.

Setting up Toolbox
A wizard helps you set up Toolbox. SolidWorks has not named this utility consistently: you will see it called Configure Toolbox or Toolbox Setup. You access the functionality by choosing Toolbox ➪ Configure; first you see Welcome to Toolbox Setup, and then Follow the steps below to configure Toolbox.

Regardless of what you actually call this wizard, you really need to be aware that the word “configure” in this setting is just an unfortunate use of terminology. It does not have anything to do with SolidWorks configurations; it enables you to use settings to control Toolbox functionality. Some of the functionality that Toolbox Setup controls happens to be related to SolidWorks configurations,
so be aware that the word configure is used multiple ways (which can lead to confusion).

Selecting your hardware — Step 1
The SolidWorks Toolbox has a huge assortment of parts, including many international hardware standards. You might consider this tool collection too much, but someone else might wonder why her favorite part is not included. This is why one of the first things you do when setting up your Toolbox is to limit your Toolbox parts to the parts that you are going to need. This has several benefits, including that users will experience less visual confusion, accessing less data from the database will improve performance, and that users will be less tempted to get creative with hardware selection, limiting themselves to hardware that is more easily attainable.

When you start setting up Toolbox, one thing you need to ask yourself is “Am I really going to use this part?” You have the option to turn off entire standards, hardware classifications, or specific types of hardware.

Using Toolbox Setup to limit hardware selections
The check boxes next to each item enable you to select and deselect that item. For example, you can turn off the entire ANSI Inch standard, just the Retaining Rings category, or any of the parts:
Basic, C-type, or E-type. In another part of the interface, you can turn off specific sizes to limit further the size of the library.

Customizing hardware — Step 2
The next step in setting up your Toolbox is to customize the hardware. Many options are available in the Toolbox Setup interface, as shown in Figure 10.12. Much of the work that you do here will be done in Excel, if you choose to go that route.

Figure 10.12 shows the top fields covered by a message prompting you to make changes to the data. If you click in the grayed out area, the message disappears, and you will have access to enable or disable specific sizes of the selected hardware, and add custom properties.

Custom Properties
If you click the Custom Property Definition icon in the Custom Properties area, the interface shown in Figure 10.13 appears and enables you to establish custom properties with a set of preset options that will display in the Toolbox PropertyManager when you place the part.

Customizing the hardware

Establish custom properties in the Custom Property Definition dialog box.

When this part is placed into the assembly, the options you created in Figure 10.13 show up when you place the part. The newly added properties integrate perfectly into the existing Toolbox interface, and make it very easy for your users to follow the established procedure without skipping steps.

Part number and description
In the Toolbox Setup interface, the Part Number, Description, and Comment fields are blank. You can fill in these sections, so when you actually create the parts, those values propagate to your Bill of Materials (BOM). The Part Number is the part number associated with the configuration properties for the BOM; it is not a custom property. The Description is a configuration specific custom property, even when you save sizes out as separate parts.

Notice that next to the bearing image at the top of the screen, a note says the part has 240 possible configurations. Does this mean you are going to enter manually 240 different part numbers and descriptions? No way. This interface has no intelligent capabilities except copy and paste. If you enter both size and type data for the 12 different kinds of hardware, you will need to enter tens of thousands of lines of data, which is obviously impractical just to implement some of the metadata in your hardware library.

To get around the manual data entry, you can export the complete table of data to Excel and build the part numbers and descriptions there. You can export the data using the button shown on the left, which is at the right end of the title row in Figure 10.12 (about halfway down on the right side of the image).

If you have a semi-intelligent part numbering system, you can build the part number based on size data exported in the table. Figure 10.15 shows an example of this type of Excel function, the result of using the Concatenate command.

Using the Excel Concatenate command

In this example, the base part number 54383-0-AAHA is assembled together with data that Excel pulls from cells E3, M3, and Q3, along with the letter H. You can find more sophisticated examples that use the Vlookup command in Excel.

By populating the part number and description fields this way, you can save a lot of data entry time and avoid mistakes. Once the data is filled in, you can import the Excel data back into the Toolbox Setup Wizard, and it populates the database for you. If you are wondering if this is a bit of a workaround, it is. However, if you want the benefits of having this data automatically entered into your BOMs, without requiring users to enter data manually, this technique, convoluted as it
is, will save you a ton of time and mistakes.

Creating parts or configurations
At this point in the Toolbox Setup Wizard, you have not yet been presented with the option to use parts or configurations. It is an absolutely pivotal decision and should probably be the first thing you do in the wizard, but it doesn’t show up until Step 3. To preview the difference between using parts or configurations, you have the option for each individual size to be either a configuration within a larger part or a separate part. So your socket head cap screws could all be contained with several hundred configurations within a single part file, or you could have several hundred individual part files where each part contains a single-size socket head cap screw. More on that decision later, but for now, assume you have already made that decision, and for what you do next, it doesn’t matter which option you decided upon.

In addition to the export and import Excel files functionality, the icon at the left also enables you to create all the parts or configurations for a given Toolbox part. The Fillister Head Screw has 7,044 possible configurations. Use this tool with care. Do you really need a single part with more than 7,000 configurations? Can you imagine how 7,000 part files in a library just for the fillister screw would affect your users?

The point is that this functionality is available if you want to try it or feel you need it, but it comes at a price. Another option that may be less insane would be to export the table data, reformat it so that it looks like a design table, trim out unnecessary data, then bring it into the library part and
create the configurations that you need.

Note
If you look at the data in the Toolbox Setup, Customize Hardware step more closely, you see that the Fillister screw contains duplicate data for cross and slotted heads, and then each of these is tripled by specifying simplified,
cosmetic, and schematic thread representations. This means that in essence you have six times as many configurations as is warranted by just the geometry itself. The rest of the configurations are due to metadata. You have to make up your mind about how to deal with this. Does your BOM need information about metadata, such as drive type, screw tip type, screw material, or finish? If this level of data is handled elsewhere such as in PDM, ERP/MRP (Enterprise Resource Planning/Material Requirements Planning), you may be able to get away with representing the geometry in the SolidWorks model. However, if the information in your SolidWorks BOMs is used to feed your PDM or ERP system, additional metadata will be required.

Regardless of how you divide it up, adding this type of data to your Toolbox is going to be a lot of work. The good news is that you’ll only need to do it once, and it is done for all your users and for all future releases of the SolidWorks software.

User Settings — Step 3
The main decision you have in Step 3 is Parts or Configurations. Many people have a superstitious fear of configurations in SolidWorks. Others are turned away by the overhead of having a single part file that contains possibly hundreds, or even thousands, of configurations get very large.

Parts or Configurations
One of the huge advantages of configurations over individual parts is that if you have a change that you want to make across all sizes, it is easy to do if you use configurations, but a veritable nightmare if you use individual parts. Granted, you won’t be making many changes to library parts, but if you need to derive a new library part from an existing one, it is the same deal, though it is much easier with configurations than with individual parts.

If I could, I would dispel users’ fear of configurations. If you plan how you are going to use the configurations, and maybe control them through a visual interface like a design table, they work reliably. For many things, they are simpler to use. Switching configurations of a part is easier than swapping parts. Figure 10.16 shows the User Settings dialog box.

One thing you need to be aware of with this choice between parts and configurations is that if you start doing it one way and then switch, you may cause yourself problems. For example, if you start using Configurations, and switch to Parts, the parts that it copies each have configurations built into them.

With the file management side of things, I recommend not making a definite choice on this parts or configurations dilemma until you have read the section on file management heading in this chapter. Configurations are very attractive, but when you are dealing with managing files and the changing nature of Toolbox parts, you have more to consider than you might originally think.

The User Settings dialog box enables you to select between parts and configurations.

Read-only settings
When you create a multi-user environment for Toolbox, Toolbox must handle part permission to ensure edits are available when they need to be. The settings shown in Figure 10.16 are the defaults, and they should remain that way. I can’t think of a reason to change the read-only settings in the User Settings dialog box.

Permissions — Step 4
The Toolbox Setup Wizard is attached to a specific database. To check on which database it is connected, choose Tools ➪ Options ➪ Hole Wizard/Toolbox. The path displayed should point to the database that this specific SolidWorks installation is attached. If this is a shared database and you create a password in the Permissions dialog box, you have taken control of the Toolbox installation
for all the users who are also linked to that database. In fact, the first user to create a password can take control. As SolidWorks Administrator, I recommend you are the first one to apply a password. The permissions only affect the settings in the Permissions dialog box, not for the rest of the settings in the Toolbox Setup Wizard.

If for some reason you are locked out of the database, replacing the database with a fresh copy should get you back in, but you will lose changes.

Smart Fasteners — Step 5
Smart Fasteners is a tremendous idea, but as it turns out, it is probably one of the weaker areas of functionality in Toolbox. Smart Fasteners has two modes of operation. The first is to simply populate all the holes in an entire assembly automatically and all at the same time. The problem with this is that little irregularities throw off the automation, so you wind up spending more time intervening manually than it saves you. The types of errors it creates will be bolts that go into holes head first, on the ends of shafts, in appropriate sizes, and so on.

The more appropriate way to use Smart Fasteners is to select a face or a set of holes and tell it to populate that smaller selection. A more guided application of this sort is a benefit when compared to manually inserting fasteners, especially the nut and washer stacks. The settings here in the Toolbox Setup Wizard Smart Fasteners page are shown in Figure 10.18.

Smart Fasteners settings in the Toolbox Setup Wizard

Adding user parts to the Toolbox library
You may run into situations where you want to add your own parts to the Toolbox library to be used similarly to how you use Toolbox parts. Adding parts is easy, but some limitations exist as to what you can do with user-added parts. You cannot use user parts for functionality such as Smart Fasteners.

Figure 10.19 shows the Design Library tab in the Task Pane, where the main Toolbox selection interface resides. Using this interface, you can add your own folders to the existing list, and then save the current part document to that folder.

The Design Library interface

Note
When adding parts to Toolbox that need to mate to other parts, it is a good idea to use Mate References. The details of applying and using Mate References can be found in the SolidWorks 2009 Bible (Wiley, 2009), which is a user guide.

File management and Toolbox
Have you ever noticed that SolidWorks example files never use Toolbox parts directly? There are reasons for that, including that not all customers have Toolbox. In addition, Toolbox is not really set up to be used “that way.” By “that way,” you can infer that file management in Toolbox is not as simple and straightforward as your other SolidWorks part data. This is where Toolbox, as a configurator
rather than a library, starts to have a negative impact. Because the files do not exist as a static collection of files, you have to handle file management for Toolbox differently.

In the final four chapters of this book, I discuss SolidWorks Workgroup PDM in detail, and include some information on using Toolbox with Workgroup PDM. In this chapter, I deal with manual file management techniques for Toolbox. You should also be aware that other PDM products exist that have special tools to handle Toolbox data specifically. This includes SolidWorks Enterprise PDMs, which is not covered in this book.

Because of the nature of the SolidWorks Toolbox, you cannot do much with manual file management of Toolbox parts. Toolbox parts need to reside in the library. Sometimes, Toolbox parts may exist in places other than the library, and at these times, you need to be careful, particularly if your Toolbox parts frequently have configurations added to them.

The case of file management when Toolbox parts are accessed from outside of the Toolbox library is much simpler if you are working with sizes as individual parts instead of configurations. If you have a copy of a part with configurations, it could easily happen that any given part in any given user’s Toolbox has configurations that another part in another user’s Toolbox does not. It is true
that since SolidWorks 2007, Toolbox can re-create missing configurations, but in certain situations this may not work (including if Toolbox happens to be turned off). I do not recommend tempting fate by depending on Toolbox in this way.

The best practice recommendation is not to send Toolbox data along with “Pack-and-Go” assemblies if the recipient of your assembly has Toolbox. Find out if people you send assembly data to do not have Toolbox, and then you should send the Toolbox parts. If possible, it is best practice to use the Create Parts setting (rather than configurations) if you send assemblies to other people to avoid completely any difficulties of file management and missing configurations.

If you have multiple copies of Toolbox parts on your computer or network drives, I recommend you delete them, or at least move them to a place that SolidWorks cannot access. The number one rule of file management with SolidWorks is that all SolidWorks documents should have unique filenames. The other side of that is that you should never have different documents with the same names. If one Toolbox part has ten configurations and another one of the same name has only  five, you have different documents with the same names.

Caution
The bottom line to this entire discussion is that when you use configurations, Toolbox is guilty of violating the most important file management rule by design. You can certainly make it work, but you have to be careful to avoid multiple copies of Toolbox parts with different configurations.

Alternatives to Toolbox
After discovering that some drawbacks exist to the Toolbox functionality, many SolidWorks Administrators ask what the alternatives to Toolbox are. Certainly you can make Toolbox work, but you may not be able to avoid using a series of progressive workarounds. You may be lucky, and your requirements may turn out to be completely compatible with the way Toolbox works, or maybe you can work around the shortcomings in some other way, using tools outside of SolidWorks to cover the data management or metadata issues.

If you’re not one of the lucky ones, and you still need a library but can live without the 70 percent functionality that Toolbox provides, the most common solution is to use Toolbox to create a library of static parts. You can still use all the automation tools to add custom properties to the parts before they are saved out. Generally, people who choose this option just use the regular library functionality.

Of course, third-party libraries exist, but you probably won’t see any additional value in them. With any library, you are going to need to do some customization work, and Toolbox gives you all the tools you need to do it.

By using an alternative to Toolbox, you are giving up the Smart Fastener integration with the Hole Wizard holes, and other Toolbox specific functionality, such as a nicer method for swapping parts.

Summary
The promise of SolidWorks Toolbox is great. It provides a very valuable list of functionality. Finding situations in which the functionality that it promises actually works as promised is the primary challenge Administrators face when establishing how it will be used at a company. You should not view Toolbox as a plug-and-play hardware library unless you are an individual user and tend not to share assemblies with other Toolbox users. Toolbox requires thought and understanding to realize its full potential and to make it work in the typical multi-user environment with a lot of file sharing.

Combining Toolbox with manual file management techniques requires either a great deal of discipline to avoid multiple copies of parts with different configurations or using copied parts instead of configurations.

Many Administrators choose to create static libraries based on parts made in Toolbox. To do this correctly, the task of creating library parts should be centralized, and a written procedure followed to make sure it is done correctly. Library documents should contain specific information, such as custom properties, tags, configurations, filenames, and so on, that conform to an established standard.