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 LinearPattern button.
   • Select the Part Design → Apply a pattern → LinearPattern 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. If no features were selected the Select feature task panel opens: select one or more (hold down the Ctrl key) from the list and press the OK button.
6. The LinearPattern parameters task panel opens. See Options for more information.
7. 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 LinearPattern from the context menu.
2. The LinearPattern 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 version 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.
• Specify the Direction of the pattern:
  • 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.
• Check the Reverse direction checkbox to reverse the pattern.
• introduced in version 1.0: Specify the length Mode:
  • Overall Length: Enter the Length from a given point on the first occurrence to the same point on the last occurrence.
  • introduced in version 1.0: Offset: Enter the Offset from a given point on the first occurrence to the same point on the next occurrence. For n occurrences: OverallLength=(n-1)*Offset.
• Specify the number of Occurrences (including the original feature).
• If the Update view checkbox is checked the view will update in real time.

Limitations

See PartDesign PolarPattern.