Hole Wizard Type PropertyManager

The Hole Wizard PropertyManager appears when you create a new Hole Wizard hole.

Two tabs appear:
  • Type (default). Sets the hole type parameters.
  • Positions. Locates the Hole Wizard holes on planar or nonplanar faces. Use dimensions, sketch tools, sketch snaps, and inference lines to position the hole centers.
You can switch between these tabs. For example, select the Positions tab and locate the holes, then select the Type tab and define the hole type, then select the Positions tab again to add more holes.
  • To add different hole types, add them as separate Hole Wizard features.
  • The available PropertyManager options depend on the hole type selected in Hole Specification.
  • You can create a custom Hole Wizard hole size by clicking Tools > Options > System Options > Hole Wizard/Toolbox > Configure and creating a customized standard.

To open this PropertyManager:

Create a part, select a surface, and click Hole Wizard (Features toolbar) or Insert > Features > Hole > Wizard .
You can also open the Hole Wizard Type PropertyManager from an assembly.

Favorite

Manage a list of styles for Hole Wizard holes that you can reuse in models. Hole Wizard Favorite saves all the Hole Wizard PropertyManager parameters of your favorite holes.
SOLIDWORKS saves your favorites per Hole Type. Select a Hole Type to list the available favorites.
Apply Defaults/No Favorite Resets to No Favorite Selected and the default settings.
Add or Update a Favorite Adds the selected Hole Wizard hole to the Favorites list.
  • To add a style, click , enter a name, then click OK.
  • To update a style, edit the properties on the Type, select the hole in Favorites, then click and enter a new or existing name.
Delete Favorite Deletes the selected style.
Save Favorite Saves the selected style. Click this option, then browse to a folder. You can edit the file name.
Load Favorite Loads the style. Click this option, browse to a folder, then select a style.

Hole Type and Hole Specifications

The Hole Specification options vary depending on the Hole Type. Use the PropertyManager images and descriptive text to set the options.

Counterbore  
Countersink  
Hole  
Straight Tap
Tapered Tap  
Legacy Hole Holes created before the SOLIDWORKS 2000 release.
Counterbore Slot Specifies slot holes of length Slot Length . Under Dimension Scheme, select Slot Length from Arc Center to Arc Center or Slot Length from Arc Tangent to Arc Tangent .
Countersink Slot
Slot
  Standard Specifies the hole standard. For example, select ANSI Metric or JIS.
  Type Specifies drill sizes, tap drills, dowel holes, or screw clearance. For example, select All Drill Sizes or Screw Clearances.
  Filter Available for PEM® Inch or PEM® Metric standards. Filters the selections available for Type.
  Size Specifies the fastener size.
  Show decimal values For straight holes or slots, displays decimal hole size values for all, letter, number, or fractional drill sizes.
  Fit (Counterbore and Countersink only.) Specifies the fastener fit: Close, Normal, or Loose.
  Show Custom Sizing Sizing options vary depending on the hole type. Use the PropertyManager images and descriptive text to set the options such as diameter, depth, and angle at bottom.
You can override the value in the boxes. To revert to the default values, click Restore Default Values. The background color of the boxes is white for the default value, and yellow for the override value.
  Configurations Specify the configuration to modify when a model has configurations requiring different Hole Wizard sizes. You can also use a design table.

Section Dimensions

(Legacy Holes only.) Double-click a Value to edit it.

End Condition

The End Condition options vary depending on the hole type. Use the PropertyManager images and descriptive text to set the options. From the list, select an end condition. To reverse direction, click Reverse Direction . Set other end condition options depending on the condition and hole type.

Blind Hole Depth (Blind only.) Set the hole depth. For tap holes, you can set the thread depth and type. For pipe tap holes, you can set the thread depth. Automatically Calculate Depth is selected by default. If you select a different hole Size under Hole Specifications, the end condition depths update automatically. If you clear Automatically Calculate Depth, the end condition no longer updates automatically if you change the Size.
You can override the value in the boxes. To revert to the default values, click Restore Default Values. The background color of the boxes is white for the default value, and yellow for the override value.
Vertex (Up to Vertex only.) Select a vertex.
Face/Surface/Plane (Up to Surface and Offset from Surface only.) Select a face, surface, or plane.
Depth to Shoulder Applies to Blind, Up to Vertex, Up to Surface, or Offset to Surface.
Depth to Tip Applies to Blind, Up to Vertex, Up to Surface, or Offset to Surface.
Offset Distance (Offset from Surface only.) Set the offset distance from the selected face, surface, or plane.

Options

The Options vary depending on the hole type. Use the PropertyManager images and descriptive text to set the options such as:

Head clearance Specifying a Head clearance value other than 0.00 adds that value above the fastener head using the document units.
Near side countersink, Under head countersink, and Far side countersink Sets diameter and angle.
Cosmetic Threads and Thread class Select a thread option:
 
  Tap drill diameter Cosmetic thread Remove thread
 
  Cuts the hole at the tap drill diameter. Cuts the hole at the tap drill diameter with a cosmetic thread.

With thread callout. Adds an annotation for drawings only.

 Cuts the hole at the thread diameter.

Feature Scope

Specifies which bodies or components you want the feature to affect.
  • For multibody parts, see Feature Scope in Multibody Parts.
  • For assemblies, see Feature Scope in Assemblies.

Tolerance/Precision

Specifies values for tolerance and precision. This section is also available for Hole Wizard features in assemblies.

Tolerance values automatically propagate to hole callouts in drawings. If you change values in the hole callout, the values update in the part. You can also vary tolerance values for configurations.

  Callout Value Select a description of the hole type, for example, Thru Hole Diameter, Near Side Countersink Diameter, and so on.
  Tolerance Type From the list, select None, Basic, Bilateral, Limit, Symmetric, and so on.
Maximum Variation Enter a value.
Minimum Variation Enter a value.
  Show Parentheses Select to display tolerances values in parentheses.
Unit Precision From the list, select the number of digits after the decimal point for the dimension value of the second unit of measurement.
Tolerance Precision Select the number of digits after the decimal point for tolerance values of the second unit of measurement.