PartDesign Mirrored/ko

A Pocket feature created from a sketch containing a circle (A) is used to create a Mirrored feature. The vertical axis of the sketch (B) is used to the define the mirror plane. The result (C) is shown on the right.

Usage

Create

1. Optionally activate the correct Body.
2. Optionally select one or more features.
3. There are several ways to invoke the tool:
   • Press the Mirror button.
   • Select the Part Design → Transformation Features → Mirror 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 Mirror 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 Mirrored object in the Tree View.
   • Right-click the Mirrored object in the Tree View and select Edit Mirror from the context menu.
2. The Mirror 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.
• Specify the mirror Plane:
  • Vertical sketch axis: The Y-axis of the sketch (the plane passes through this reference and the Z-axis of the sketch, only available for sketch-based features).
  • Horizontal sketch axis: The X-axis of the sketch (idem).
  • Construction line #: A separate entry for each construction line in the sketch (idem).
  • Base XY-plane: The XY-plane of the Body.
  • Base YZ-plane: The YZ-plane of the Body.
  • Base XZ-plane: The XZ-plane of the Body.
  • Select reference…: Select a planar face in the 3D View.
• If the Recompute on change checkbox is checked the view will update in real time.

Properties

Data

Base

• 데이터 (Hidden)Originals (LinkList): A list of selected features. Will be ignored, if the 데이터Transform Mode property is set to Whole shape.
• 데이터Transform Mode (Enumeration):

  Features

  Whole shape (default)

Mirrored

• 데이터Mirror Plane (LinkSub): Mirror plane

Part Design

• 데이터Refine (Bool): Default is True. Refine shape (clean up redundant edges) after operations.
• 데이터Fuzzy Tolerance (FloatConstraint): Default is -1.0. Fuzzy tolerance:

  If value > 0: use the value

  If value = 0: leave default value

  If value < 0: determine value

Transformation

• 데이터Suppressed Indices (IntegerList): Indices of pattern instances that are suppressed. introduced in 26.3

Limitations

• See PartDesign PolarPattern.
• Be careful when mirroring PartDesign Hole features or a body that contain modeled threads since right handed threads become left handed (and vice versa) in the mirrored portion.