Manufacturing

Tool Time

5 Jan, 2004 By: Greg Jankowski


SolidWorks Toolbox is a collection of common components that can be shared with other users. For a successful Toolbox implementation, you must configure and set up Toolbox so that others within your organization can share a common library of components.

SolidWorks Toolbox can be purchased separately as an add-on product and is also included as part of SolidWorks Office and SolidWorks Office Professional. Two add-ons are available from the Tool/Add-in dialog box: SolidWorks Toolbox and the SolidWorks Toolbox Browser. Toolbox Browser adds the PropertyManager used to add components to an assembly. SolidWorks Toolbox adds some productivity tools to the Toolbox drop-down menu-for example, bearing calculator, beam calculator, structural steel, and grooves.

What's in the Toolbox
Toolbox provides a set of components that are configurable via a menu of attributes such as size, length, and thread length as well as values for those attributes. Toolbox uses a database to drive the creation of additional configurations within the SolidWorks documents.


Figure 1. Toolbox dialog for a finished hex bolt

Toolbox also lets you use Smart Fasteners to populate and size fasteners for selected holes, or auto-populate all holes, within an assembly. With Smart Fasteners you can also define the top and bottom stack so that bolts, screws, and washers can be inserted in one step.


Figure 2. Top and bottom stack configuration

Before you install SolidWorks Toolbox, consider how the parts will be used, what type of components need to be available, and who will use them. Toolbox offers a wide range of components and provides the ability to add your own components to the library. This is done via the Toolbox/Add My Parts Wizard. This Wizard imports a set of components into Toolbox for reuse.

During the Toolbox implementation, you should also define the catalogs, chapters, and pages that need to be available. If your organization does not use catalogs (ANSI, JIS, ISO, etc.), chapters (washers, screws, pins, etc.), or pages (countersunk head, hex head, etc.), deselect the Enabled checkbox for the appropriate area. This limits the selections you see when using the Toolbox Browser.

Default values for the components can be defined using custom properties. This can be a text input cell or drop-down list of predefined selections. Users can define the attributes for either a group or individual components. Define these properties under the Toolbox/Configure Browser/Custom Properties dialog box.

Share the Toolbox
Toolbox can also be configured for a multiuser environment. First, you need to establish the file system attributes of the shared Toolbox directory. This is a common directory accessed by all users.

Follow these steps to set up Toolbox for use in a multiuser environment:

  1. Install the Toolbox parts and database to a network location accessible by all users.
  2. Configure the Toolbox installation to define the available content by reducing the standard list and adding your own components. Review and define the custom properties for the components.
  3. Set the shared Toolbox parts directory (for example, Toolbox Parts\Browser or C:\Program Files\Common Files\SolidWorks Data\Browser), all subdirectories, and components to read-only mode. You can do this with Windows Explorer. Select the Toolbox parts (Browser) directory, right-click, and select Properties. On the General tab, select Read-only. Go to the Advanced tab to ensure that all subfolders and files are also changed. Select Apply. Check one of the part attributes within one of the subdirectories to insure the change was made.
  4. Make sure all users can access the Toolbox directory. Do this by sharing the folder or, preferably, placing the directory on a network drive.
  5. All users should point to the same shared Toolbox parts directory. This is done via the TOOLBOX.INI file located in the \Toolbox\ directory. The ToolboxPartFolder option should point to the shared Toolbox parts directory.
  6. Set the document properties within the Toolbox/Customize Browser/Document Properties page:
    1. Copy Part File = No copy
    2. Read-Only Status = Insert documents as read-only
    3. Writing to Read-Only Document = Always change read-only status of documents before writing
  7. Set the Don't Prompt To Save Read-Only Reference Documents option in the Tools/Options/External References dialog box. If you use PDMWorks to manage your documents, you have the option to set directories that don't require revision control. SolidWorks Toolbox parts typically do not require revision control.

SolidWorks software, starting with SolidWorks 2004, marks Toolbox files with an attribute to identify these types of parts. This is done with all Toolbox content. If you add new components to Toolbox or have legacy data, you can also mark Toolbox content with a utility found at \Toolbox\Data Utilities\SLDSETDOCPROP.EXE. Select the Toolbox directory and update the document property.

When you update to a new release or service pack, you may also need to update the Toolbox database and files. After an update, review the information in the Toolbox update log file, DATABASEUPDATEERRORS.LOG, for issues.

Successful sharing
You can use SolidWorks Toolbox to easily set up and share common components within your organization. When using Toolbox in a multiuser environment, take some time to ensure the setup is consistent and that it points to a common location.


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