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Create

1. Optionally activate the correct Body.
2. Optionally select one or more features in the Tree View or the 3D View.
3. There are several ways to invoke the tool:
   • Press the Polar Pattern button.
   • Select the Part Design → Transformation Features → Polar Pattern option from the menu.
4. If there is no active Body, and there are two or more Bodies in the document, the Active Body Required dialog will open and prompt you to activate one. If there is a single Body it will be activated automatically.
5. The Polar Pattern Parameters task panel opens. See Options for more information.
6. Press the OK button to finish.

Edit

1. Do one of the following:
   • Double-click the PolarPattern object in the Tree View.
   • Right-click the PolarPattern object in the Tree View and select Edit Polar Pattern from the context menu.
2. The Polar Pattern Parameters task panel opens. See Options for more information.
3. Press the OK button to finish.

• Choose the mode:
  • Transform body: Transforms the whole base feature's shape (default). introduced in 1.0
  • Transform tool shapes: Transforms the individual tool shapes of selected features.
    • To add features:
      1. Press the Add Feature button.
      2. Select a feature in the Tree View or the 3D View.
      3. Repeat to add more features.
    • To remove features:
      1. Press the Remove Feature button.
      2. Do one of the following:
         • Select a feature in the Tree View or the 3D View.
         • Select a feature in the list and press the Del key.
         • Right-click a feature in the list and select Remove from the context menu.
      3. Repeat to remove more features.
    • If there are several features in the pattern, their order can be important. See Ordering features.
• Axis:
  • Press the button to reverse the direction of the pattern.
  • Specify the axis reference:
    • Normal sketch axis: The Z-axis of the sketch (only available for sketch-based features).
    • Vertical sketch axis: The Y-axis of the sketch (idem).
    • Horizontal sketch axis: The X-axis of the sketch (idem).
    • Construction line #: A separate entry for each construction line in the sketch (idem).
    • Base X-axis: The X-axis of the Body.
    • Base Y-axis: The Y-axis of the Body.
    • Base Z-axis: The Z-axis of the Body.
    • Select reference…: Select a Datum Line in the Tree View or a Datum Line or edge in the 3D View.
  • introduced in 1.0: Specify the angle Mode:
    • Extent: Enter the total Angle (wrongly labeled as Length). If the angle is less than 360°, the occurrences are evenly distributed from 0° (first occurrence) to the given angle (last occurrence). If the angle is 360°, the occurrences are evenly distributed around the circle. For n occurrences an angle of 360° is equivalent to an angle of 360°*(1-1/n).
    • introduced in 1.0: Spacing: Enter the Spacing angle from a given point on the first occurrence to the same point on the next occurrence. For n occurrences: TotalAngle=(n-1)*Spacing.
  • Specify the number of Occurrences (including the original feature).
• If the Recompute on change checkbox is checked the view will update in real time.

If some of the selected features are additive and others subtractive, their order can have have an impact on the final result. You can change the order by dragging individual features in the list.

• Any shape in the pattern that does not overlap the parent feature will be excluded. This ensures that a PartDesign Body always consists of a single, connected solid.
• The PartDesign patterns are not yet as optimized as their Draft counterparts. So for a large number of instances you should consider using a Draft PolarArray instead, combined with a Part boolean operation. This may require major changes to your model as you are leaving PartDesign and therefore cannot simply continue with further PartDesign features in the same body. An example is shown in this Forum topic.
• A pattern cannot be applied directly to another pattern, be it polar, linear or a mirror. For this you need a PartDesign MultiTransform.