Mirror Feature

Creates a copy of a feature, (or multiple features), mirrored about a face or a plane. You can select the feature or you can select the faces that comprise the feature.

• Bodies to Mirror. Select a body in a single model or multibody part to create a mirror entity.

• Multibody parts. Apply features to one or more multibody parts by selecting Geometry Pattern and using Feature Scope to choose which bodies should include the feature.
  
  

You must create the model to which you want to add the features for multibody parts prior to adding those features.

• Sheet metal features. You can mirror these individual sheet metal features:

• • Base-flange/tabs

  • Closed corners

  • Edge flanges

  • Hems

  • Mitered flanges

If you modify the original feature (seed feature ), the mirrored copy is updated to reflect the changes.

To mirror a feature:

1. Click Mirror on the Features toolbar or Insert, Pattern/Mirror, Mirror.

2. Under Mirror Face/Plane , select a face or a plane in the graphics area.

   You can select features, the faces that comprise features, or a body with multibody parts.

• To use features: Under Features to Mirror , click one or more features in the model or use the flyout in the FeatureManager design tree.

• To mirror the entire model: Under Bodies to Mirror , select a model in the graphics area.

  The mirrored model attaches to the face you select.

• To use faces: Under Faces to Mirror , in the graphics area click the faces that comprise the feature you want to mirror. Faces to Mirror is useful with imported parts where the import process included the faces of the feature, but not the feature itself.

• To mirror a pattern on multibody parts:

1. Under Features to Mirror , select the pattern from the FeatureManager design tree.

2. Under Options, select Geometry pattern.

3. Under Feature Scope, specify which bodies you want the feature to affect.

• To use bodies: Under Bodies to Mirror , in the graphics area select the body you want to mirror.

3. If you select Bodies to Mirror, the following Options appear:

• Merge solids. When you select a face on a solid part, and clear the Merge solids check box, you can create a mirrored body that is attached to the original body, but is a separate entity. If you select Merge solids, the original part and the mirrored part become a single entity.

• Knit surfaces. If you select to mirror a surface by attaching the mirror face to the original face without intersections or gaps between the surfaces, you can select Knit surfaces to knit the two surfaces together.

  

4. If you want to mirror only the geometry (faces and edges) of the features, rather than solving the whole feature, select Geometry Pattern .

   The geometry pattern option speeds up the creation and rebuilding of the pattern. However, you cannot create geometry patterns of features that have faces merged with the rest of the part.  To mirror a feature pattern on multibody parts, you must select Geometry Pattern.

   The geometry pattern is only available with Features to Mirror and Faces to Mirror.

5. To mirror the visual properties of the mirrored entities (SolidWorks colors, textures, and cosmetic thread data), select Propagate Visual Properties.

6. Click OK .

Related Topics

Mirror Entities

Mirror Part