Sketch the 2D profile on the right plane

Front plane for revolves (cup, anything radially symmetric). Top plane for extrudes (pin, goal, toggle — anything with a flat base footprint). Use a vertical centerline for revolves; the centerline becomes the axis of revolution.

Apply dimensions until the sketch is fully defined

Onshape shows under-defined geometry in blue. As you add dimensions, more lines turn black (fully defined). Dimension every length, diameter, and angle that the manual specifies. For dimensions the manual doesn't specify, use the team's estimates (in the per-element sections of this page).

Run the operation (revolve, extrude, or loft)

Revolve for radially symmetric shapes (cup). Extrude for prismatic shapes (pin sections, goal walls, toggle). Loft for shapes that change cross-section over height (the pin's tapered middle).

Verify dimensions with the Measure tool

Before exporting, use Onshape's Measure tool to confirm bounding-box dimensions match the manual. If anything's off, fix the sketch — don't patch in the export.

Export STEP and document in the notebook

Right-click part → Export → STEP, units in millimeters. Save with a clear name (e.g., Override_Cup_Placeholder_v1.step). Drop into the team's Drive in 2026-27 Override / CAD / Game Elements. Document the verified-vs-estimated dimensions in your notebook (see Section 8).

Create the document

Onshape → Create → Document. Name it Override_Cup_Placeholder_v1. Open the default Part Studio.

Sketch the half-profile on the Front plane

Click the Front plane in the feature tree → Sketch (S key). Draw the right half of the cup's outline (matching the SVG above), with a vertical centerline along the Y-axis as the axis of revolution.

Apply dimensions

Lock the sketch with these dimensions: vertical axis 164.5 mm, bottom horizontal 40 mm, top horizontal 40.1 mm, waist Y-position 55 mm, waist X-position 29.5 mm. Sketch turns black when fully defined.

Revolve 360°

Exit sketch → Revolve. Select the closed sketch region as the face, the vertical axis line as the axis. Type: Full (360°). The cup appears as a solid hourglass.

Shell to hollow

For more realistic fitment behavior, hollow the cup. Shell tool → select the top circular face as the face to remove → thickness 2.5 mm → direction inward.

Verify with Measure

Before exporting, use the Measure tool: confirm top OD = 80.2 mm, waist OD = 59 mm, total height = 164.5 mm. Fix the sketch if any value is off.

Export STEP

Right-click the part → Export → format STEP → units Millimeter → filename Override_Cup_Placeholder_v1.step.

Create the document and sketch the bottom hex

New document Override_Pin_Placeholder_v1. Open Part Studio. Sketch on Top plane → Polygon (regular) tool → 6 sides → flat-to-flat 35.6 mm.

Extrude the bottom flange

Exit sketch → Extrude → Blind, depth 16.2 mm → New solid. This is the bottom flange.

Sketch the top hex (on the top face of the flange)

Click on the top face of the flange → Sketch. Draw a hexagon, flat-to-flat 80.3 mm, centered on the same axis. Don't extrude yet — this is the lower profile of the loft.

Sketch the upper hex (on a parallel plane offset by 74.5 mm)

Create a new plane parallel to the Top plane, offset 74.5 mm above the flange's top face. Sketch a hex flat-to-flat 80.3 mm on this plane (same as the lower profile — the taper isn't literally tapered to a smaller dimension, the manual shows it transitioning to the same outer profile but with a different visual style).

Note: If you want the taper visible, offset the upper hex by ~5 mm and adjust. For placeholder purposes, parallel-up is fine.

Loft between the two hex sketches

Loft tool → select the lower hex sketch as profile 1, the upper hex sketch as profile 2. Operation: New solid (or Add to existing). This produces the tapered middle section.

Extrude the top section

Sketch on the top face of the loft → hex flat-to-flat 80.3 mm → Extrude Blind 74.3 mm. This is the top wider section.

Combine and verify

Use Boolean → Union to combine the three solids if they aren't already merged. Then use Measure to verify total height = 165 mm and the three hex flats match.

Export STEP

Right-click → Export → STEP → Millimeter → Override_Pin_Placeholder_v1.step.

Create the document and sketch the base profile

New document Override_Goal_Alliance_v1. Open Part Studio. Sketch on Top plane → draw a 142.5 mm square centered on origin. Use Fillet tool with R = 81.9 mm at each corner (note: this radius is larger than the square's half-side, so corners blend into a near-circular shape — that's correct).

Extrude the base footprint

Exit sketch → Extrude → Blind, depth 10 mm (the manual shows a thin bottom layer). New solid.

Sketch the top profile (on a plane offset to alliance height)

Create a new plane offset 72.5 mm above the Top plane (Alliance goal: 82.5 mm total height − 10 mm base layer). Sketch a square 88.8 mm with R81.9 corners on this plane. This is the top profile.

Loft from base profile to top profile

Use Loft between the bottom face of the base footprint (or the original sketch) and the upper square sketch. This creates the trapezoidal frustum.

Cut the receptacle hole on top

Sketch on the top face → circle Ø60.1 mm centered on the origin. Exit → Extrude → Operation: Remove → Through all (or 37.8 mm depth). This creates the cup/pin receptacle.

Duplicate for short neutral and tall center

Save the alliance goal as STEP. Then either: (a) duplicate the document and edit the offset plane to 136.5 mm (short neutral height − 10 mm) for the second goal, then 212.7 mm for the tall center; or (b) parameterize the height in a configurations table and let Onshape generate all 3.

Export each as STEP: Override_Goal_Alliance_v1.step, Override_Goal_ShortNeutral_v1.step, Override_Goal_TallCenter_v1.step.

Create the document and sketch the triangle

New document Override_Toggle_Placeholder_v1. Open Part Studio. Sketch on Front plane (so the prism extrudes horizontally) → draw an isosceles triangle: base 30.2 mm wide along the X-axis, apex 51.6 mm above the base midpoint.

Extrude 660.2 mm

Exit sketch → Extrude → Blind, depth 660.2 mm. The result is a long triangular prism — that's the toggle.

Verify and consider rounded corners

Use Measure to confirm 51.6 / 30.2 / 660.2. The real toggle has slight rounding on the edges (~5 mm fillet); for a placeholder, sharp edges are fine. If you want more accuracy, apply a small Fillet on the three long edges of the prism.

Export STEP

Right-click → Export → STEP → Millimeter → Override_Toggle_Placeholder_v1.step.

Create the assembly

In your team's Hero Bot Onshape document → Insert tab → New Assembly. Name it HeroBot_V1_Assembly.

Insert the Hero Bot parts

Insert the drivetrain and manipulator parts you've already CAD'd. Mate them together using Fastened mates (the manipulator base is fixed to the chassis at a specific position).

Insert game elements

Insert the cup, pin, and at least one alliance goal from the STEP files you exported. Position them at expected match locations: a goal centered in front of the robot for scoring, a cup near the manipulator pickup zone, a pin in the loading area.

Run the manipulator through its range of motion

Use Mate values to drive the manipulator's revolute joints through their full angle range. Watch for collisions with the goal, the cup, or the chassis. Any collision is a design problem to fix.

Check critical clearances

For each goal size (alliance 82.5 mm, short neutral 146.5 mm, tall center 222.7 mm), confirm: (a) the manipulator can reach the receptacle from a reasonable robot stance, (b) the gripper has 5–10 mm clearance around the cup at placement, (c) the arm doesn't hit the goal's rounded corners during approach.