learndesign.tech Search

Case study: modelling with sketches (bike bracket)

· Fox Bright

Fusion's Model from Sketch sample, step by step. Two-sided extrude to an object, symmetric extrude from the mid-plane, projecting a circle onto a face, mirroring a feature, a fillet, and a mass check at the end.

A finished mountain-bike rocker arm bracket in Fusion with a bore through one end and a counterbore mirrored on both sides.

This is a mountain bike rocker arm, a bracket that gives the rear suspension its pivot. Fusion provides the sketches; you add the features. It is a good exercise in reading instructions one step at a time and in the difference between the ways an extrude can end.

The reference for this case study is Autodesk’s own Tutorial: Modeling with sketches in the Fusion help. Its four activities are condensed below; the full write-up, with a screenshot for every click, is on that page. The video follows the same steps. Keep one of them open beside Fusion.

The drawing

The sketches in the sample already carry these dimensions, so you will not type many of them. Read the drawing anyway. It tells you what the finished part should look like from each side, and it is what you check your model against at the end.

The finished part

Orbit it, section it, or use the measure tool in the viewer to compare with yours.

Open and save

Data panel → home → Samples → Basic Training → 04 Modeling → 04 Model from Sketch. Save As somewhere you own; the sample folder is read-only.

Activity 1. The body: a two-sided extrude to an object

Select the main profile, everything except the innermost circles (hold Shift; zoom in if a profile is hard to pick). Extrude. Direction: Two Sides. For each side, extent To Object, and click the end point of the sketch line that marks where that side should stop, not the rectangle. No numbers typed; the sketch already knows. Afterwards, turn Sketch1 and Sketch2 back on in the browser; Fusion hides a sketch once you have extruded from it.

Fusion extrude dialog with direction Two Sides and the rocker arm profile highlighted in blue
Two-sided extrude with both extents set To Object, ending on the two sketch lines.

Activity 2. The rear boss and its bore

Select the larger of the two circular profiles at the end, with its centre circle, and extrude Symmetric, 20 mm total, Join. Model symmetric parts from their mid-plane whenever you can; both sides stay equal and you only manage one number.

Then the bore:

  1. Right-click Sketch1, Edit Sketch. Add a 10 mm circle at the centre (C, snap, type 10). Finish.
  2. Press P for Project, pick the outer face of the boss as the sketch plane, then click the new circle. It appears on the face in purple.
  3. Extrude that circle as a Cut, extent To Object, click the far face. Straight through.

The point of projecting rather than just sketching a new circle: it stays tied to the original sketch. Change the 10 there and the bore follows.

Activity 3. The counterbore: same trick, then mirror

Edit Sketch1 again, add a 24 mm circle at the other end. Project it onto that outer face. Extrude the ring between the projected circle and the smaller one as a cut, -10 mm.

Fusion extrude dialog set to cut with distance -10 mm on a red highlighted ring profile
The counterbore cut, 10 mm deep, from the projected circle.

Now Mirror (S, type mirror). Object type Features, pick that extrude-cut from the timeline, mirror plane = the origin plane through the middle of the part. Turn the Origin folder on if you cannot see it. Both sides now match, and they will keep matching.

Activity 4. The slot and the fillets

Select the bottom rectangle sketch and PressPull it through the whole part. PressPull turns into an Extrude cut on its own; on an edge it would have become a Fillet. Then select the two inside corner edges, press Q, and fillet at 5 mm.

Fusion fillet dialog with two inside edges of the rocker arm selected
A 5 mm fillet on the inside corners finishes the part.

Everything you built hangs off Sketch1 and Sketch2. Edit a dimension there, or in Modify → Change Parameters, and the whole part updates without touching a single feature.

Check the mass

In the browser, expand Bodies, right-click the body and set Physical Material to Steel if it is not already. Right-click the body again and choose Properties. The mass should read 559.358 g (0.559 kg if Fusion shows kilograms).

If yours is different, work backwards. Too heavy: the bore or the slot did not go all the way through, or the counterbore was not mirrored. Too light: the boss was extruded one way instead of symmetric 20 mm, or a cut went deeper than it should. A missing 5 mm fillet changes the mass by only a few grams, so it will not explain a big gap.

Share it

Save the design, then use Share → Public link (the share icon at the top right of Fusion, or right-click the design in the Data panel). Turn the link on and copy it. Anyone with the link can orbit the model in a browser without Fusion.