Your First Part in Onshape

In this lesson you build one real part from start to finish: a flat mounting plate with two holes and rounded corners. Plates and spacers like this hold sensors, motors and electronics on almost every FTC robot, so the steps you practise here are the same ones you will use all season. Follow along in your own document; reading is not enough, your hands need to learn where the tools are.

Step 1: Create the document

1. 1
   Create

   Sign in to Onshape, click Create and choose Document. Name it with your team number and Practice plate.
2. 2
   Check units

   Open the document menu (top left) and choose Workspace units. Set length to millimetres so every number you type means the same thing.
3. 3
   Rename the tab

   A new document opens a Part Studio tab. Right-click the tab at the bottom of the screen, choose Rename and call it Plate.

Step 2: Learn to move around

Step 3: Sketch with dimensions and constraints

1. 1
   Start a sketch

   Click the Top plane in the feature list, then click Sketch. Press N to look straight at it.
2. 2
   Draw the outline

   Choose Center point rectangle and click on the origin first, then drag out a rectangle. Starting on the origin keeps the plate centred.
3. 3
   Dimension it

   Choose Dimension (shortcut D), click the top edge, place the number and type a width. Do the same for a side edge. Practice values such as 60 mm by 30 mm work well.
4. 4
   Place hole centres

   Use the Point tool to place two points inside the rectangle. Add a Horizontal constraint between them, then dimension the distance between them and from one point to the origin.
5. 5
   Check the colour

   When every line and point turns black, the sketch is fully defined. Click the green check mark to close the sketch.

Step 4: Create a variable, then extrude

A variable is a named number you can reuse in any feature. Instead of typing the plate thickness in three places, you type it once. Click the Variable tool in the toolbar, name it thickness and give it a value such as 4 mm. The variable must sit above the features that use it in the feature list.

1Variable:      thickness = 4 mm
2Extrude depth: #thickness
3Fillet radius: #thickness / 2
4Hole points:   the two sketch points from Step 3

1. 1
   Extrude

   Select the sketch region, click Extrude, keep New selected and type #thickness as the depth. Confirm with the green check.
2. 2
   Add holes

   Click Hole, choose Simple and select the two sketch points as locations. Pick a diameter (a practice value such as 5 mm is fine here) and set the end to Through.
3. 3
   Round the corners

   Click Fillet, select the four short vertical edges at the corners and type #thickness / 2 as the radius. Rounded corners are safer to handle and stronger when 3D printed.

Now test your design: double-click the variable in the feature list and change it to 6 mm. The plate should get thicker and the fillets larger, with no red errors. Then change the width dimension in your sketch. If anything breaks, the sketch was probably not fully defined, so go back and fix it. A part that survives changes like this is said to have good design intent.