Components

Remind them of Stage 1C: they drew a master layout sketch (wheelbase, tube centerlines, key reference points). Today we turn those lines into actual 3D parts. The big idea: we don't model parts in isolation, we drive them off the layout. Onshape calls its workspace a Part Studio; in Fusion the equivalent concept is one design file holding multiple Components and Bodies. Stress that a good layout means edits propagate everywhere automatically.

This is the #1 confusion for beginners coming from solid-modeling tutorials. A Body is just a lump of geometry. A Component is the FRC unit you care about — a gusset, a tube, a gearbox plate — it has its own origin, can hold multiple bodies, and is what you apply Joints to. In Onshape every part lives in a Part Studio; in Fusion you deliberately create Components. Tell them: if it's a separate physical part you'd hold in your hand, make it a Component.

Demo live: right-click the top of the browser, New Component, leave 'Empty' checked, double-click to rename. The single most common Fusion mistake is modeling everything into one component because they never noticed the active-component dot. Show them: whatever has the dot is where geometry goes. Make them rename BEFORE modeling — Component1, Component2 is unmaintainable on a real robot.

This IS in-context modeling. Instead of typing dimensions, they reference the layout. Demo: activate Drive_Rail_L, create sketch on the XY plane, hit P, click the layout lines for that rail. Projected geometry shows purple and is associative — if the layout moves, this updates. This is the Fusion answer to Onshape's 'derive from layout' habit. Common mistake: redrawing lines by hand instead of projecting, which kills the whole single-source-of-truth benefit.

Now the part becomes 3D. Tie every dimension to reality: 2x1x0.100 tube, 2x1x0.0625 if light, 1/4in gusset plate. In the Extrude dialog point out the Operation dropdown (New Body) and that it builds inside the active component. Common mistake: extruding a tube as a solid block — show them the thin-wall / shell or sketching the hollow rectangle so it's a real tube. Reinforce: CAD that doesn't match orderable stock can't be built.

This is the Onshape Variables translation. Open Modify > Change Parameters, add User Parameters at the top. Then in any dimension box they can type wallThk instead of 0.1. Powerful demo: change wallThk from 0.1 to 0.0625 and watch every tube thin out. Tell them to parameterize the values they'll second-guess: wall thickness, plate thickness, hole patterns. Don't over-parameterize trivial stuff — that just adds clutter.

Housekeeping that pays off. Demo renaming and dragging Appearance (G) onto bodies — color-coding makes a 40-part robot readable. Ground the chassis frame so it can't drift when they start adding Joints (next lesson). Grounding is the Fusion equivalent of Onshape's 'fix' — without it, the whole assembly can float when solved. Common mistake: leaving Component12, Body3 names everywhere, then nobody can find anything during build season.

COTS = commercial off-the-shelf. The Onshape crowd uses the MKCad library; in Fusion we download vendor STEP/F3D files (REV MAXSwerve, WCP gearboxes, AndyMark wheels) and Insert them. Fusion also has a built-in McMaster-Carr inserter for hardware. Show inserting a STEP and that it comes in as its own component. Rule: if a vendor sells it, don't model it — insert it and spend your time on custom parts. For gears you actually need, the SpurGear add-in generates 20DP teeth correctly.