In this exercise, you will be modeling a sort of flat game piece manipulator. This mechanism features live-axle compliant wheels, a belt reduction, and tube plugs.
Tube Plugs
Tube plugs are a great way to build simple and robust structures.
Many vendors including WCP, REV, Andymark, and Last Anvil offer in various tubing sizes.
They can be used to connect plates to the open face of tubes or to connect tubes to each other without the use of a gusset.
Tube Plugs
Tube plugs can be used to create gusset-less tube to tube (left) and tube to plate (right) connections. (Photo Credits: FRC 4414, FRC 9442)
This exercise also introduces you to the use of the the Assembly Mirror Featurescript which is a useful tool to help make your assembly more parametric.
Make sure to add this to your Featurescripts if you have not already.
Part Studio Instructions
Navigate to the "Exercise #1 Part Studio" tab in your copied document and follow the instructions in the slides to complete the part studio for this exercise.
0. Final Part Studio.
1. Create the layout sketch on the Right plane. Begin by sketching the tube profiles.
2. Using the Origin Cube functions you learned previously, sketch the pulleys and belt. This is a 5mm pitch 12T to 30T transmission with a 70T belt.
3. Finish the layout sketch by sketching a 60 mm circle to represent the motor and a 2" circle for the intake wheel.
4. Create the tube sketch plane by using an offset mate connector reference.
5. Sketch the tubes by tracing over the layout sketch. There should be no dimensions in this sketch.
6. Extrude the lower and use tube converter to turn it into a thin-wall 1x1 with a 0.5" hole spacing pattern. We will create the upper tube in a later step.
7. Create the plate sketch on the outside face of the 1x1 tube. Begin by sketching the bearing hole and motor bore hole.
8. Sketch the 2" bolt circle for mounting motor. You can utilize the Origin Cube variable for a #10-32 clearance hole by typing #10_32 into the dimension and selecting the #Clearance_Fit_10_32 variable. Use a Circular pattern to pattern the hole sketch. Although we pattern the hole 6 times, we set three of them to construction geometry as we only need 3. Set the left most hole to be coincident with the centerline between the pulleys.
9. Sketch the mounting holes by using a linear pattern. The tube holes are 0.196" in diameter (A #10-32 "close fit") so we will use the same size for the plate.
10. Finish the plate sketch by drawing the plate outline around the sketch features.
11. Extrude the plate to be 1/4" thick.
12. Create the pocketing sketch on the outside face of the plate. Sketch ribs to connect the mounting points.
13. Use the Part Lighten Featurescript to pocket the plate. We use 3/16" rib and wall thickness, and 0.26" tool diameter.
14. You may have noticed in the previous step that the pocketing created some unsightly bumps along the outside contour as a result of the mounting holes. We will make these edges smooth with a simple trick in the next slide.
15. Open the pocketing sketch and sketch two lines spaced exactly half the pocketing wall thickness away from the outer edge of the mounting hole (NOT the center of the circle). In our case, this would be half of 3/16". This "tricks" the Part Lighten Featurescript by creating an extra rib where the bumps would have been.
16. Edit the Part Lighten feature to include the two new ribs. The pocketed part should no longer have the bumps.
17. To create a reference for extruding the upper tube, we use the Mirror feature to mirror the plate across the Right plane. Since we do not want to actually use this component in the assembly, we can change the color of the part and add zREF to the part name so that it will appear at the very bottom of the part list when inserting parts in the assembly.
18. In the assembly, we would like the location of the two plates to be fully parametric. Since Onshape does not support assembly mirroring, we can instead use the Assembly Mirror Featurescript which provides a workaround to assembly mirroring by generating a pair of mate connectors to simulate an assembly mirror. The featurescript will generate a mate connector at the origin of the selected part, and another at the center of the virtually mirrored part. The usage of these two mate connectors will become clear when we create the assembly.
19. Using the tube sketch we created earlier in the part studio, we can now extrude the upper tube profile up to the mirrored plate's inside face. This ensures that the upper tube is parametric to changes in intake width.
20. Convert the solid into a 2x1 thin-wall tube with 0.5" hole pattern spacing.
21. Create the bottom polycarbonate plate on the top face of the bottom tube.
22. Model the roller shaft with the Shaft Featurescript. You can estimate the length first and then adjust it once you create the assembly.
23. Model the belt using the Belt & Chain Gen Featurescript. Use a mate connector offset from the plate's bearing hole as the reference plane and offet by 3/8". Select the layout sketch pulley PDs to use as the guides.
24. Finish the part studio by naming your features and organizing them into folders. Assign the part materials accordingly.
Assembly Instructions
Next, navigate to the "Exercise #1 Assembly" tab in your copied document and follow the instructions in the slides to complete this exercise.
0. Final assembly.
1. Insert all of the part studio components, except for the zREF part, and group the plates and tubes with the origin cube. Fasten the cube to the origin.
2. Copy the side plate and use the mate connectors generated by the Assembly Mirror Featurescript to fasten the plate into place. The location of the "mirrored" plate is fully parametric as the mate connectors generated by the Featurescript will automatically update when changes to the plate occur.
3. Insert the upper tube plugs and make a copy of the lower tube. Fasten all the components to their correct locations.
4. Insert the motor and roller pulleys. Fasten them into place and then fasten the roller shaft.
5. Fasten the belt to the roller pulley. Double check that the motor pulley is properly lined up with the belt.
6. Insert and fasten the Configurable Spacer Stack and flex wheel. The spacer stack is a configurable assembly that will automatically calculate the optimal stack of spacers to fill a gap. While this functionality is not used for this exercise, it will be very useful in later exercises. When fastening the Spacer Stack assembly, make sure to select the pre-generated mate connectors on each end and NOT the spacer body.
7. Use the Linear Pattern feature to pattern the spacer and wheel.
8. Copy the Spacer Stack and modify it to be 0.5" long, then fasten it into place to finish the roller.
9. Insert, fasten, and replicate 3/16" rivets from MKCad to attach the plate to the lower tube.
10. Insert, fasten, and replicate 0.5" long #10-32 bolts from the Standard Content Library for attaching the the tube plug on the upper tube.
10. Insert, fasten, and replicate 1/2" long 10-32 boltwashers from MKCad for shaft retention.
11. Insert, fasten, and replicate 0.5" long #10-32 bolts from the Standard Content Library for attaching the motor.
12. Insert, fasten, and attach 1.5" long #10-32 bolts from the Standard Content Library for attaching the polycarb panel. Also add #10-32 thin jam nuts from MKCad Library.
13. Finish your assembly by organizing the parts into folders and naming your replicates.
Verification
If all is done correctly your assembly should have 32 Instances.
Parametric Modeling
Some of the steps we took to complete this exercise could have been simplified.
For instance, we didn’t necessarily need to use the Assembly Mirror feature for the plate.
We didn’t need to use an “Up to face” extrude for the upper tube.
However, we practice these techniques because, while they may marginally increase modeling time upfront, they can save significant amounts of time when going back and editing.
CAD is an iterative process — your models and designs won’t be perfect the first time around, so making your model easier to modify and more robust to changes (e.g., changing the width of this intake) will save you time and effort in the long run.
As you use best practices, they’ll become second nature.
Tweaking Your Model
Try playing around to get a feel for what things are and aren't parametric in exercise 1. You can try changing things like the width, length, tube positions, or gear ratio. Which dimensions are easy to change and which are difficult? Which dimension changes cause rebuild or assembly error?
