PartDesign SubtractiveHelix

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

Usage

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

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

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 * PartDesign SubtractiveHelix dialog.png

Axis
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.

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

Pitch
The distance between turns in the helix.

Height
The height of the helix (center-center).

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

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

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

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

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

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


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


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