PartDesign LinearPattern/cs

The PartDesign LinearPattern tool creates a linear pattern of one or more features.

An L-shaped pad (B) made on top of a base pad (A, also referred to as support) is used for a linear pattern. The result (C) is shown on the right.

Usage

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 Linear Pattern button.
   • Select the Part Design → Transformation Features → Linear 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 Linear 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 LinearPattern object in the Tree View.
   • Right-click the LinearPattern object in the Tree View and select Edit Linear Pattern from the context menu.
2. The Linear Pattern Parameters task panel opens. See Options for more information.
3. Press the OK button to finish.

Options

• 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 PartDesign PolarPattern.
• Direction:
  • Press the button to reverse the direction of the pattern.
  • Specify the direction 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 length Mode:
    • Extent: Enter the Length from a given point on the first occurrence to the same point on the last occurrence.
    • introduced in 1.0: Spacing: Enter the Spacing from a given point on the first occurrence to the same point on the next occurrence. For n occurrences: Extent=(n-1)*Spacing.
  • Specify the number of Occurrences (including the original feature).
• Direction 2: Idem. introduced in 1.1
• If the Recompute on change checkbox is checked the view will update in real time.

Limitations

See PartDesign PolarPattern.