PartDesign PolarPattern

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PartDesign PolarPattern.svg PartDesign PolarPattern

Menu location
Part Design → PolarPattern
Default shortcut
Introduced in version
See also


The polar pattern tool takes a selected feature and creates a set of copies rotated around a chosen axis. Starting with v0.17, it can pattern multiple features.

PartDesign PolarPattern example.png

Above: a slot-shaped pocket (B) made on top of a base solid (A, also referred to as support) is used for a polar pattern. The result (C) is shown on the right.

How to use

  1. Select the feature(s) to be patterned. Alternatively, the feature can be selected from a dialogue after step 2.
    v0.16 and below Only a single feature can be selected, and it must be the last one at the bottom of the feature tree.
  2. Press the PartDesign PolarPattern.png PolarPattern button.
  3. v0.17 and above Press Add feature to add a feature to be patterned. The feature must be visible in the 3D view:
    1. Switch to the Model tree;
    2. Select in the tree the feature to be added and press spacebar to make it visible in the 3D view;
    3. Switch back to the Tasks panel;
    4. Select the feature in the 3D view; it will be added to the list.
    5. Repeat to add other features.
  4. v0.17 and above Press Remove feature to remove a feature from the list, or right-click on the feature in the list and select Remove.
  5. Define the axis. See Options.
  6. Define the angle between the last copied occurrence and the original feature.
  7. Set the number of occurrences.
  8. Press OK.


Polarpattern parameters.png


When creating a polar pattern feature, the PolarPattern parameters dialogue offers different ways of specifying the pattern rotation axis.

Normal sketch axis

An axis being normal to the sketch and starting in the origin of the sketch of the feature being used is taken as axis for the polar pattern.
The pattern direction can be reversed by ticking 'Reverse direction'.

Horizontal sketch axis

Uses the horizontal axis of the sketch for axis.

Vertical sketch axis

Uses the vertical axis of the sketch for axis.

Custom Sketch Axis

If the sketch which defines the feature to be patterned also contains a construction line (or lines), then the drop down list will contain one custom sketch axis for each construction line. The first construction line will be labelled Sketch axis 0.

Base (X/Y/Z) axis

v0.17 and above Select one of the Body Origin's standard axis (X, Y or Z) as axis.

Select reference...

Allows you to select either a DatumLine or an edge of an object or a line of a sketch to use for axis.

Angle and Occurrences

Specifies the angle to be covered by the pattern, and the total number of pattern shapes (including the original feature). For example, four occurrences in an angle of 180 degrees would give a spacing of 60 degrees between patterns. There is one exception: If the angle is 360 degrees, since first and last occurrence are identical, four occurrences will be spaced 90 degrees apart.