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A parametric piping bag tip

· Fox Bright

A 3D-printable icing nozzle where the number of teeth, the wall thickness and the diameter are all parameters. Loft, thicken, emboss, circular pattern, pipe.

A grey cone-shaped piping nozzle in Fusion with 25 fine triangular teeth around the bottom edge and the parameters dialog open.

An icing nozzle is a cone with a shaped opening. The shape of the opening is the texture of the icing. Commercial ones come in sets; I wanted one file where you change a number and get a different tip. The number that matters most is how many triangles are cut around the rim, from two big ones to twenty-five tiny ones.

Research first

Look at real nozzles: some have a flat closed face with a shaped hole, most have an open cone with teeth cut into the edge. Look at a 3D-printed one. Watch someone pipe with one. Notice the rim at the top that stops the nozzle sliding out of the bag. Those observations become the design intent: open cone, cut teeth, top rim, everything adjustable.

Parameters

Save the file first. Then S → para → Change Parameters, and add as you go:

  • bottom_dia 20 mm, the tip opening
  • height 40 mm
  • thickness 1 mm, the wall
  • num_triangles 6, no units
  • base_length = bottom_dia * pi / num_triangles, the width of one tooth so that they exactly fill the circumference
  • triangle_offset 0.5 mm, how far the teeth are pushed down

Add comments to each one. Future you will not remember what triangle_offset was for.

The cone

  1. Sketch a circle on the ground plane, snapped to the origin, dimensioned to bottom_dia.
  2. Offset plane from the ground by height. Sketch a circle on it, diameter bottom_dia * 1.5.
  3. Loft between the two circles, the orange surface loft, not the solid one. You want an infinitely thin cone so you can control the wall in the next step.
  4. Thicken the surface inwards by thickness. If you typed 1 mm, right-click the feature in the timeline and Edit Feature to replace it with the parameter. Don’t undo; edit the history. That habit is what makes the model parametric.

The teeth

  1. Sketch on a vertical plane through the origin. Draw a rough triangle below the origin.
  2. Constrain it: Equal on all three sides, so it stays equilateral, and Midpoint between the base and the origin, so it is centred.
  3. Dimension the base to base_length.
  4. Emboss (S → emboss). Sketch profile = the triangle, faces = the inside of the cone, effect Deboss, depth -thickness. Because the wall was thickened at an angle, the triangle floats a little above the bottom edge; set the vertical distance to -triangle_offset to push it down through.
Fusion emboss dialog with a triangle profile projected onto the inside of a cone
Emboss wraps the flat triangle onto the cone and cuts through the wall.
  1. Circular Pattern, type Features, select the emboss, axis = the vertical axis, quantity num_triangles.
Close-up of triangular teeth cut around the bottom of the nozzle in Fusion
Six teeth patterned around the rim. Changing num_triangles changes both the count and the tooth width.

The rim

Edit the top circle’s sketch and Offset the circle outward by thickness. Finish, then Pipe along that edge with section size thickness, operation Join. Thicker wall, thicker rim.

The finished nozzle in Fusion with a rounded rim at the top and the parameters dialog
The pipe tool makes the rim that keeps the nozzle in the bag.

Then break it

Change thickness to 2 mm: if the teeth vanish, the emboss depth was typed rather than parametric. Change num_triangles to 2, 3, 8, 25. Adjust triangle_offset for each; big teeth want more, fine teeth want almost none. The first version of base_length divided by a typed 6 instead of num_triangles, which only showed up when I tried 2. Testing the extremes is how you find those.