Using the Solidworks Toolbox

This guide describes the initial steps on how to set up, access and use the team's common hardware toolbox in Solidworks! This guide was written by Austin Tailon Huang , so send me a message if you have any questions .

Set-up Guide

Enable the toolbox add-in in Solidworks. Everyone whos using a license from the UW should have access to this add-in . When you start solidworks, click:
1. Tools → Add-Ins → Activate Solidworks Toolbox Library and Solidworks Toolbox Utilities on start up.
Make sure that you've downloaded the latest push from GrabCad.
Back up and rename your local Solidworks Data file. This file is typically stored in C:/SOLIDWORKS Data/. I renamed mine to "SOLIDWORKS Data (Local)", but as long as its not named "SOLIDWORKS Data" anything is fine!
Open the the General System Options by clicking the Cog icon.
Click the [...] icon to change the Hole Wizard and Toolbox folder. The shared toolbox folder is the "SOLIDWORKS Data" folder in /Mars Rover 2022 Mechanical/Documentation/Toolbox Database/.
1. Check the box to make this the default folder location.
2. Also, while you are here check the box to lock concentric mates for Toolbox components .
Click "OK" to save the changes.
To access the toolbox in Solidworks, click the "Design Library" icon and hit the toolbox icon. Right now, libraries are saved for ANSI Inch, ANSI Metric, PEM Inch and PEM Metric hardware components.

Troubleshooting with GrabCAD

There is a very real possibility that you will run into issues when downloading toolbox files from GrabCAD. Just to provide some background information, whenever you insert a new variation of a toolbox component that has never been used before, it adds a new configuration to the host part. For example, shown below is the host part file for a regular hex nut. When I insert a 5/8-11" hex nut from toolbox for the first time, it will generate a configuration in the part named "HNUT 0.6250-11-D-N".
However, for some reason every time you make changes to the host file of any toolbox part, the "read-only" status of the part gets checked - I've tried to find a way to disable this, but I have had no luck and have since given up.
The implication of this file property is that whenever someone in GrabCAD creates a new configuration of any part that differs from the current local version of the part you have saved, you may run into an issue where the file in question is unable to be downloaded from GrabCAD as it is labelled as "read-only".
To bypass this error, you need to go to the toolbox folder, right click and select "properties on the folder", TURN OFF the "read-only status" and apply changes to the folder, subfolder and files. After doing that, you should be able to download the files from GrabCAD. If changing the read-only status of the folder doesn't work, you may need to individually change the read only status of all the parts creating errors in GrabCAD, but selecting the entire folder should do the trick.
I will admit, this is quite the inconvenient error. However, eventually once we generate all the configurations for pieces of hardware we use, this issue should become quite rare.

Inserting Toolbox Components

You can individually insert any piece of hardware just by dragging and dropping it into your assembly, then selecting the correct configuration. When you drag in the component, you will be given the option to select critical dimensions. Before you finish configuring the component, take time to assign a part number and description. This step is very important, as when you generate a bom for an assembly toolbox components will generate their assigned part numbers and descriptions. By default, these are unassigned so please make sure you assign this information for toolbox components.
In this example I have inserted in a 1" long, 1/4-20 socket head cap screw. Currrently, we order most of our fasteners from McMaster, so when configuring this fastener, I have pulled the part number and part description from the McMaster catalogue page.
When inserted into the assembly, toolbox components will be labelled as their file name and configuration. I think this way is pretty easy to read, as you know its a socket head cap screw from file name, and from configuration name you know its a hex drive, 1/4-20 thread 1in long with 1in threaded length.
- However, if you want to change how toolbox components are displayed in the feature manager, click: System Options - General → Hole Wizard/Toolbox → Configure. This opens the toolbox settings page. Click "3 - Define user settings" and you can change what shows up in the FeatureManager and BOM accordingly. Make sure that the file name is used for feature manager, part number is used as part number in BOM, and description is used as description in BOM and that "Create Parts" is selected for new fastener sizes.
  - You will need to log into the toolbox settings to save any changes. If so, the password is "uwrobotics"
You can also configure the part number and description for toolbox components directly in the Toolbox settings page. Aside from clicking "configure" as described above, you can also access toolbox settings just by searching your computer. Click "2 - Customize Hardware". Scroll to your desired hardware, and input the information as necessary. IMPORTANT NOTE: I really don't recommend entering the part numbers this way, as there are tens of thousands of configurations for some part types. It's easy to enter the part number on the wrong configuration, so you are better off to assign part numbers when inserting components.

Using Smart Fasteners (Example)

To get started, click the "Smart Fasteners" button in the assembly tab, and click "OK" to the pop up.
Smart fasteners rely on using hole features made using the hole wizard, so ensure that any holes in your parts have been properly defined using the hole wizard tool. In this example, we will look at a simple example where there are four 10-32 screws (red) that go into tapped holes, and two 4-40 screws (blue) that will use a washer (for this example).
Lets start with the 10-32 screws. Click the hole feature and click "Add" to create a series of fasteners for the 10-32 screws. Smart fasteners will automatically select the fastener type, length and diameter.
If you want to change the fastener type, click "Edit Grouping" and select the series grouping you just placed. Right click it, select "Change Fastener Type" and then select any fastener you desire. For this example, I will change these fasteners to button heads.
After changing the fastener type, select the same series and click "Edit Fasteners". You can address any issues that came with fastener sizing. When I switched to button head, the automatically selected fastener length wasn't at the end of the plate. No problem, all you need to do is deselect "Auto update length" and update the fastener length to be as desired. I'm happy with these fasteners, so I will select the green checkmark to confirm the series.
Now, I'll do the 4-40 screw stack. Using the instructions described above, I created a new series for the two 4-40 screws. However, they are facing the wrong side. Why is that? Well, take a look at the plate's mating assembly. The rectangular plate has the clearance holes for 4-40 screws, and the curvy plate has the tap holes for the 4-40 screw. Smart fasteners know that in a plate assembly, the head of the bolt needs to be on the clearance hole side for the two parts to be mated, and thus it will generate the stack in the correct orientation!
To add a washer to this screw stack, all you need to do is click "add to top stack" and select your washer type. Top stack refers to all extra components near the head of the bolt, and bottom stack refers to any additional fasteners at the end of the bolt. The smart fasteners will recalculate the screw length to ensure it uses a size with enough threads of engagement, however sometimes their calculation is off. If the length is wonky, all you need to do is manually adjust the fastener length like explained before.
For one last example, say a second curvy plate is to be mated to the first using a bolt and nut in this #6 clearance hole. I'll set up a smart fastener for this hole as described above. However, since both holes are clearance holes on these plates, you can actually configure which side the head of the fastener faces by clicking "Edit Grouping". Open the grouping, right click the series then select "Flip".
To configure the nuts, select "Edit Fasteners" and this time click "add to Bottom Stack" and select a desired nut. Manually adjust bolt length if necessary and you are good to go!

University of Waterloo Robotics Design Team

Using the Solidworks Toolbox

Set-up Guide

Troubleshooting with GrabCAD

Inserting Toolbox Components

Using Smart Fasteners (Example)

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