PartDesign SubtractiveHelix

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PartDesign SubtractiveHelix
PartDesign → Create a subtractive feature → Subtractive helix
Workbenches
PartDesign
Default shortcut
None
Introduced in version
0.19
See also
Additive Helix

Description

The SubtractiveHelix tool modifies a solid by sweeping a selected sketch or 2D object along a helix path cutting away the material.

The profile (B), is swept around axis (A) in order to produce the helical groove (C) in the pre-existing work piece

Select the sketch to be swept into a helix. A face on the existing solid can alternatively be used.
Press the SubtractiveHelix button.
Set the Helix parameters (see next section).
Inspect the Helix in the view window, to ensure that the parameters do not result in a self intersecting helix.
Press OK.

When creating a SubtractiveHelix, the Helix parameters dialogue offers several parameters specifying how the sketch should be swept.

This option specifies the axis about which the sketch is to be swept.

Vertical sketch axis: selects the vertical sketch axis.
Horizontal sketch axis: selects the horizontal sketch axis.
Construction line: selects a construction line contained in the sketch used by the Helix. The drop down list will contain an entry for each construction line. The first construction line created in the sketch will be labelled Construction line 1.
Base (X/Y/Z) axis: selects the X, Y or Z axis of the Body's Origin;
Select reference...: allows selection in the 3D view of an edge on the Body, or a datum line.

This controls what parameters will be used to define the helix, Allowable choices are: Pitch-Height, Pitch-Turns and Height-Turns.

The distance between turns in the helix.

The height of the helix (center-center).

The number of turns in the helix. Define as Height/Pitch

The rate at which the radius of the helix increase along the axis. Allowable range: [-89°, +89°].

If checked, the turning direction of helix is reversed from default clockwise to counterclockwise.

If checked, the axis direction of helix is reversed from default.

If checked, the result will be the intersection of the swept profile and the preexisting body.

If checked, the helix will be shown in the view, and updated automatically on every change of the parameters.

Below are properties which can be defined after creation of the feature.

DataPitch: The axial distance between two turns.
DataHeight: The total length of the helix (not accounting for the extent of the profile)
DataTurns: The number of turns (do not need to be a whole number)
DataLeft Handed:
DataReversed: true or false. See Reversed.
DataAngle: The rate at which the radius of the helix increase along the axis. Allowable range: [-89°, +89°].
DataReference axis: The the helix axis
DataMode: The helix input mode (pitch-height, pitch-turns, turns-height)
DataOutside: If true, the result will be the intersection of the swept profile and the preexisting body.
DataHas Been Edited: If false, the tool will propose an initial value for pitch based on the profile bounding box, so that self intersection is avoided.
DataRefine: true or false. If set to true, cleans the solid from residual edges left by features. See Part RefineShape for more details.
DataProfile: Either a sketch containing a closed contour, or a face.
DataMidplane: Not used.
DataUp to face: Not used.
DataAllow multiple face: Not used.