1D: Design Methodology - Simple Swerve Drivebase

Deriving Layout Sketches and Part Modeling

Now that you have created the layout sketch, you can begin modeling the individual parts. The critical dimensions of the parts, such as the length of the tubes, will be driven by the layout sketch. This way, the tubes will automatically update with any changes in the size of the drivebase in the layout sketch.

Instructions

Start by creating a new folder tab in your Document called Drivetrain. Then, create a new part studio called Drivetrain within the Drivetrain folder. Follow the instructions in the slides to complete the part studio. Remember that the Origin Cube should be the first feature in your part studio.

1. Start by inserting the origin cube. Then, use the `Derived` tool to insert the layout sketches you previously drew from the Master Sketch part studio. This feature will automatically update if changes are made to the layout sketch.

2. Use the `Extrude Individual` and `Tube Converter` Featurescripts to model the tubes. The 2"x1" tubes should be 1/8" wall for strength, while the 2"x2" tube can be 1/16" wall.

3. Start with one corner of the bellypan. The corner is cut out to create room for the swerve module.

4. Use the Fillet sketch tool to add a 1" radius sketch fillet on the two internal corners of the cutout.

5. Next, use the Circular Pattern sketch tool to pattern the other three corners. Extrude the bellypan to be 1/8" thick.

6. Use the `Fillet All Edges` Featurescript to add a 0.25" radius fillet to the remaining edges on the bellypan by selecting the bottom face of the bellypan.

7. Add the seed instances of the holes for the bellypan.

8. Next, use the Linear Pattern sketch tool to pattern the holes along the edge.

9. Use the Circular Pattern sketch tool to pattern the holes about the origin onto all four edges.

10. Use the Linear Pattern sketch tool to pattern the holes for the 2"x2" tube.

11. Clean up the sketch by moving the dimensions so that they are all visible. A clean sketch is important for readability of the CAD so that it is easily editable in the future.

12. Extrude the holes into the bellypan. If the sketch is correctly drawn, you should not need to select each individual hole.

13. Finally, name your sketches and organize them into a folder in the feature tree. Additionally, set the material of the bellypan to Aluminum 6061 and name your parts.

Derive Feature

In this section, you were introduced to the Derived feature. This feature is extremely powerful and can be used to import parts from one part studio into another to enable references for modeling. However, you must be careful to not overuse this function as it can significantly slow down your part studios.

Feature Tree Organization

At this point, you should be feeling more and more comfortable with Onshape modeling and using Featurescripts. Always make sure to clean up your feature tree while working to keep it organized and easy to use. You can more learn about feature tree organization on the Feature Tree Best Practices page.