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Helical Boss/Base and Helical Cut

Sweeps a closed profile along a helix about an axis to add material (Helical Boss/Base) or remove it (Helical Cut), for threads, springs and worms.

Features tab > Helical Boss/Base or Helical Cut, or Insert > Boss/Base > Helical… or Insert > Cut > Helical….

The Helical page beside a part with a helical cut.

Creating a Helical Feature

  1. Sketch the closed profile and a centerline for the helix axis in one sketch, the profile clear of the axis.
  2. Select the sketch.
  3. Click Helical Boss/Base or Helical Cut.
  4. Set the Pitch and Revolutions.
  5. Click OK or press Enter.

With no sketch selected, a sketch that is the last feature in the design tree and is not used by a feature is taken as the profile. You can also select it after the page opens.

Profile

Sketch
The sketch with the closed profile.

Axis

Axis

The helix axis. Select one of:

  • a centerline or line in the profile's sketch. A solid line chosen as the axis is left out of the profile.
  • a linear edge.
  • a cylindrical face, or a circular edge, for its axis (right-click > Select Axis).
  • X axis, Y axis or Z axis.

Left empty, the sketch's first centerline is used. The text under the buttons shows which axis is used.

Helix

Pitch
The advance along the axis per turn. Default 5 mm, or 0.25 in in an inch part. Accepts an equation or a variable name.
Revolutions
The number of turns. Default 3.
Left hand
Turns the helix left-handed. Off, it is right-handed.
Reverse direction
Advances against the axis's direction.

The profile must not touch the axis, and its length along the axis must be less than the pitch.

Run-out

Run out at the end
Continues the end of the sweep straight along the helix tangent.
Length

The run-out's length. Optional:

Value Run-out
Empty A Helical Cut runs until the profile is clear of the model; a Helical Boss/Base runs one pitch
A length That length

A Helical Cut thread on a shaft with Run out at the end on, the groove leaving the shaft along the helix tangent.

Output

Operation
Join adds the helical feature to the bodies it touches. Cut removes it from every body it passes through. Intersect keeps only what each body it overlaps has in common with it. New body makes it a separate body. A feature that still has its automatic name is renamed to match, for example Boss-Extrude1 to Cut-Extrude1. An Intersect feature cannot be patterned or mirrored.

When a Helical Feature Fails

The page shows the reason. Common causes:

  • No axis is selected and the sketch has no centerline.
  • The profile touches the axis.
  • The profile is longer along the axis than the pitch, so neighboring turns would overlap.
  • A Helical Cut with a run-out and no Length has no body to run out of.

See Also