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Rotational slicing in Fusion

· Fox Bright

Draw one section, revolve two discs, pattern the section around an axis and cut every slot with one Combine. A vase, a lampshade or a sculpture from a single sheet.

A tree-shaped form made of jagged laser-cut slices arranged around a central axis with two supporting discs.

I saw a laser-cut vase built from flat slices spinning around a centre axis and wanted to try it in Fusion. It comes down to three tools: Revolve for the top and bottom discs, Circular Pattern for the slices, and Combine to cut all the slots at once. Every part comes out of the same 3 mm sheet.

Parameters first

Two of them, under Modify → Change Parameters:

  • thickness = 3 mm. Our plywood is 2.8 mm and the laser takes about 0.1 mm; rounding up gives a fit that goes together without a mallet.
  • count = 15, no units. The number of slices around the axis. You will change this later, so do not type 15 anywhere else.

Sketch one section

New sketch on the front plane. The vertical axis through the origin is the axis of the whole object.

  1. Start the section away from the origin, not on it. The gap between the section and the axis becomes the hole in the middle. I used 15 mm from the axis and a 50 mm wide base.
  2. Draw a vertical construction line (press X) up the axis and dimension it to your target height, 150 mm here. It is just a ruler.
  3. Draw the profile of the section. Mine is jagged and abstract. Yours can be a vase, a shade, whatever you want to see repeated.
  4. Draw two rectangles for the support discs, each thickness tall, crossing the section near the bottom and near the top. Add a line across the section where each disc should cut into it, roughly halfway across the overlap, and make it vertical with a constraint. That line defines the slot depth.
Fusion sketch of a jagged section profile with two thin horizontal rectangles
One section with the two disc rectangles crossing it. The rectangles are the material thickness tall.

Extrude, revolve, pattern, combine

  1. Extrude the section profile (including the little slot regions) symmetrically by thickness, whole length. Symmetric puts the sketch plane in the middle of the slice, so the discs intersect it evenly. New body.
  2. Revolve each disc rectangle around the centre axis as a new body. Select the profile first with a long press if the little slot region will not pick, then open Revolve.
  3. Check the Bodies folder: three separate bodies, nothing joined by accident.
  4. Circular Pattern, type Bodies, select the section, axis = the centre axis, quantity = count.
  5. Combine: target = the top disc, tools = every slice, operation = Cut, and tick Keep Tools. Repeat with the bottom disc as the target.
Green preview of fifteen jagged slices patterned around a vertical axis in Fusion
Circular Pattern spinning the section around the axis. Count is a parameter, so 15 can become 12 or 20 in one edit.

Hide one slice and look: the disc has a notch for every slice and each slice has a notch for the disc. Both halves of the half-lap are there, so the assembly can only go together one way.

Then play

Turn the section sketch back on and drag things. Move a disc rectangle up or down and the slot depth and disc size follow. Pull points on the profile and every slice updates. Change count. If a change breaks the pattern (a slot that no longer crosses the section), edit the sketch to fix it. The tree in the hero image is the same file with a few points pulled around.