Hole Wizard Overview

You can use the Hole Wizard to create customized holes of various types.

Creating and Deleting Hole Wizard Features

To create hole wizard holes, create a part and select a surface, click Hole Wizard (Features toolbar) or Insert > Features > Hole > Wizard, set the PropertyManager options, and click .

Hole Wizard features contain two sketches. The first sketch is the hole position sketch and the second sketch is the hole profile sketch.

When you delete a Hole Wizard feature, you can retain the hole position sketch. In the Confirm Delete dialog box, clear the Delete absorbed features option to delete only the hole profile sketch and keep the hole position sketch.

To delete the hole position sketch, select Delete absorbed features.

The Hole Wizard user interface includes the following capabilities:

Dynamic Updating

The hole type you select determines the capabilities, available selections, and graphic previews. After you select a hole type, you determine the appropriate fastener. The fastener dynamically updates the appropriate parameters. Use the PropertyManager to set the hole type parameters and locate the holes. In addition to the dynamic graphic preview based on end condition and depth, graphics in the PropertyManager show specific details, as they apply to the type of hole you select.

Capabilities

You can create these types of Hole Wizard holes:
  • Counterbore
  • Countersink
  • Hole
  • Straight Tap
  • Tapered Tap
  • Legacy
  • Slots

When you create a hole using the Hole Wizard, the type and size of the hole appears in the FeatureManager design tree.

You can create holes on a plane with the Hole Wizard, as well as holes on planar and nonplanar faces.
On models with multiple features, you can add hole wizard holes to any of the features in the model.



Holes on a plane allows you to create holes at an angle to the feature.

Face Selection

You can select a face before (preselection) or after (postselection) clicking Hole Wizard on the Features toolbar.
  • If you preselect a planar face, the resulting sketch is a 2D sketch.
  • If you postselect a planar face, the resulting sketch is a 2D sketch unless you first click 3D Sketch.
  • If you preselect or postselect a nonplanar face, the resulting sketch is a 3D sketch.

Unlike a 2D sketch, you cannot constrain a 3D sketch to a line. However, you can constrain a 3D sketch to a face.

Sketch Selection

In the PropertyManager, on the Positions tab, under Hole Positions, you can click Existing 2D Sketch and select an existing 2D sketch to position and automatically create the holes at all endpoints, vertices, and points of the sketch geometry. You can select sketch entities like lines, rectangles, slots, and splines.

Sketch Options specify the geometry used to automatically create the instances.
  • Select Create instances on sketch geometry to use sketch geometry to place the holes.
  • Select Create instances on construction geometry to use construction geometry to place the holes.


Favorite Name

For each hole type (except Legacy), you can create, save, update, or delete hole types to include your favorite properties parameters. This allows you to apply any saved hole types to a SOLIDWORKS document.