Customise And Convert Toolbox As A Standard Component​

Customise and convert toolbox as a standard component

If you are looking for an entire library of standard components to model with, look no further as SOLIDWORKS Toolbox is here to save the day. It is a library of standard components used to automate and standardise the use of pre-defined components like fasteners (bolts, nuts, washers, etc). SOLIDWORKS Toolbox is included as an add-in within SOLIDWORKS Professional and Premium.

So, let’s jump in and see how we can use this amazing tool to customise our toolbox components, create custom hardware and also how to convert our toolbox components to standard SOLIDWORKS part files.

Section 1: Customise Toolbox

Since Toolbox is fully integrated with SOLIDWORKS CAD you can simply drag and drop the desired components from the design library section on your Task pane.

 1. Turn on your toolbox add-in:

  2. Design Library Tab:

Once the Toolbox add-in is turned on you can access the toolbox components from the design library tab. Toolbox supported standards include ANSI inch & metric, ISO, AS, DIN, GB, IS, JIS, KS, etc. The library is filled with lots of hardware components like bearings, bolts and screws, nuts and washers, pins, keys and many more that you can simply drag and drop in your assembly design.

Once you insert the toolbox component on the assembly window, the “configure component” properties tab gets activated which lets you change the properties like size, length, thread display and add comments, part number and descriptions to show on the BOM list.

However, sometimes you might not find the appropriate size that fits your design.

Don’t worry, with the use of toolbox settings we can customise these components to create new sizes that are not included in the database. You can also specify materials, add custom properties and other details required.

Please Note before making any changes:

  1. Make sure you have a backup database just in case if any issues arise to your custom database or if your toolbox is stored on a Network drive.
  2. Try not to modify an existing Standard. Recommended option is that you create a copy of the standard you wish to use and add your customisations to that copied standard.

  3. Configure Toolbox You can access the toolbox settings directly from the design library panel by clicking on the icon shown below:

Or you can also search and launch from the windows search bar “Toolbox Settings 20XX”.

The toolbox settings contain 5 steps to configure Toolbox.

  1. Hole Wizard:

In this step you can define the settings for Hole Wizard; select the standards by checking the tick box that you want to include and from within each standard you can define the hole types and sub-types that are available.

    2. Customise Hardware

Like Hole wizard, in this 2nd section you can select the hardware standards that you want to appear in your toolbox library by checking the tick box. This option enables the users to limit the standard components that can be accessed which could save time in searching the components and by reducing these unwanted datasets we are making our updates go much faster.

In addition to that, users can modify the standard properties of these components located inside the folders, which includes description, part number and comments.

Again, it is best recommended to make a copy of the standard folder and make changes on the copied one to keep the standard data preserved. To do this, you need to simply right mouse click on any standard folder from the list on the left and click copy and paste.

 If you wish to add your own file on the specific hardware folder, you can right mouse click on the folder and click on Add file and select the component from your saved directory.

In the general tab on the standard properties section, you can change the description, file name of the component and enable or disable from the library.

Users can enable or disable the specific sizes for the selected component within the Size tab. You can delete a size or modify the dimensional values from each column.

With the add icon, you can create your custom size component on the list by filling the values.

Under the length tab you have the option to set the overall length of the fastener and thread length.

If you have created a custom size fastener, you will have to set the length value and thread data for it.

Under Thread data you can configure the size and thread diameter.

Users also have the option to control the thread display between cosmetic, schematic or simplified.

Recommended option is to set it as simplified only as this helps in reducing the rebuild times if you are working on large and complex assemblies.

Applying custom properties for a toolbox component:

Custom properties can be added to the component which can be edited or deleted later. Any applied custom properties value will be displayed for the component on the list.

In addition to that, configuration details can be exported to excel to enable the modification of the Toolbox components and after making few changes it can be imported back into the toolbox with the option shown below:

   3. Defining User settings:

By default, with the fresh installation of toolbox, each configuration has only Default configuration and they are all located in your SOLIDWORKS Data 20XX folder in your installation directory.

With the user settings, the user has three options to choose from which defines how the toolbox components are stored in the directory.

   a)  Create Configuration:

This option allows users to create multiple configurations on the toolbox part based on the size created. The commonly used component can have a lot of configurations and this can result in an increase in file size which can have a huge impact on the performance (rebuilt time).   So, it is best recommended to limit the size or use the next step.

   b) Create Parts:

This option will create new Toolbox components for every size created. The new component will be added on the specific directory you set on the “User settings” in the section – “Create Parts in this folder:” and they are relatively smaller in file size, which is more likely to aid in better performance when working in large level assembly design.

   c) Create parts on Ctrl+drag:

This option gives you flexibility to have a part or create configuration based on how you import the component on the design window.

Within all these options, users also have settings to control the display options for components on the assembly window.

   4. Setting Permissions

This gives user control over making changes on the toolbox settings by setting up a password.

   5. Smart Fasteners

This section has settings for Smart fasteners which can be used to automatically apply the toolbox components based on the holes created.

With the use of smart fasteners, users can select their custom toolbox from the following steps:

SOLIDWORKS Development team are working with the functionality to be able to use the top and bottom stacks (like washers, nuts, etc.) from your custom library in the series components list.

Once every setting has been changed, to save the changes you must click “Save” on the top of the settings toolbar. This will update your toolbox database and add new sizes to the components you created and save the settings you have applied.

Section 2: Convert toolbox component as a standard part.

Sometimes you might want to make the toolbox component as a regular part for editing and sharing with other users. This section outlines the steps followed in this conversion process.

If you see the Feature manager design tree on an assembly document, any toolbox component when inserted shows a Toolbox flag icon before the file name. This toolbox component can be saved on your own file location, but it will still have an internal reference which defines it to be a Toolbox part.

To make it a regular part file and remove the toolbox flag icon you need to use an application that is available in your SOLIDWORKS data utilities folder.

Folder access directory: C:\Program Files\SOLIDWORKS Corp20XX \SOLIDWORKS \Toolbox \data utilities

Application: sldsetdocprop.exe

Once you run the application the Set Document Property window opens.

The next step is to add the files (from the directory where the toolbox component is saved). If you hit the show selected property at this stage, you should get the following dialogue box:

Which means it is a standard toolbox component.

Now for conversion, you need to set the document property as No and hit update status.

After that, the show selected property window shows that the part is no longer a toolbox component.

Before you open your assembly, please make sure you have the following settings ticked off:

You can close the window and go back to the assembly and load the files and check its status.

You will find the toolbox components as a normal SOLIDWORKS part file which can be edited and shared with other users.

SOLIDWORKS Toolbox contains millions of standard hardware items, ready to be used and customised to company specific requirements. Modelling efficiency can be achieved by easily dragging and dropping the components into your design, which is fully integrated with SOLIDWORKS CAD AND SOLIDOWRKS PDM. To ensure consistency and get the most out of it, Toolbox needs to be configured and deployed correctly.

Hope with the help of this blog, you can efficiently configure your toolbox. If you have any questions, please do not hesitate to contact our Technical Support team at or through our national number.

Written by Bibek Bhurtel – Applications Engineer (Perth)

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