SolidWorks

Using the Hole Wizard

16 Feb, 2004 By: Greg Jankowski


When using fasteners within a design, you need to make sure that the corresponding holes match the fasteners you select. This gets more complicated with different kinds of holes, such as countersunk, tapped, and counterbored. You know what types of fasteners you want to use, but you also need to know what types of holes fit them.

Hole wizard at work.

Figure 1. SolidWorks Hole wizard at work.

The Hole wizard in SolidWorks helps automate this process by inserting the right type of hole based on the selected fastener. Figure 1 shows component holes created using the Hole wizard with the Hole Series option described below. The advantage of this method is that the geometry of the hole is created based on all the options for the selected features (figure 2). Each feature is tied parametrically to the selected fastener so if the fastener type changes, the hole geometry automatically updates.

Hole wizard dialog box.

Figure 2. Hole wizard dialog box.

Hole Wizard
The Hole wizard is a database-driven, intelligent user interface for creating holes within parts and assemblies. These holes consist of the following types: counterbore, countersink, hole (simple holes), tap, legacy (holes created using the old version of the Hole wizard), and Hole Series for assembly features.


Here are the steps to create a hole using the Hole wizard:
1. Select the desired face
2. Start the Hole wizard, as described below
3. Select the hole type and define the parameters
4. Dimension and constrain the hole locations
To insert a hole feature, select a face and then the Hole Wizard icon. Or select Hole Wizard from the Insert/Features/Hole menu and then select the face. The difference between preselecting and postselecting the face is the type of sketch (2D or 3D) created to define the hole location(s).

Without preselect.

Figure 3. When you select the face makes a difference in the type of sketch created. Selecting the face before you start the Hole wizard results in a 3D sketch (above). Selecting the face after you start the wizard yields a 2D sketch (below).

Postselecting the face

Figure 3 shows the difference between a preselected and a postselected face. The reason this is important is that dimensioning a 3D object can be different from dimensioning a 2D object. You can place a point-to-point dimension to create the shortest distance in horizontal or vertical orientation. A 3D sketch just dimensions the shortest distance between the two points. In most cases, it’s easier to create the hole using the preselect method so that a 2D sketch results.

When the Hole Wizard dialog box comes up, select the hole type and characteristics. Then select the standard, screw type, size, and end condition—the Hole Wizard updates the remaining parameters. Figure 2 shows a counterbored hole made for a #10 binding head machine screw. This hole type was saved as a favorite. You can define favorites for each hole type—counterbore, countersink, etc.. Select Add to include a favorite, Delete to remove one, and Update to modify an existing favorite’s configuration. The Hole Wizard defaults to the last hole the next time you access it.

Next, define the location for the hole(s). This sketch contains sketch points that define the origin of one or more holes. More than one location can be defined, as shown in figure 4, which also shows the dimension used to constrain the design. Additional constraints were placed between the points so that four dimensions could fully constrain the sketch.

Dimension the hole sketch.

Figure 4. Locate and dimension the hole sketch.

My preference is to add the constraints first and then the dimensions. After you select the point, as in figure 4, the related constraints are displayed. The point shown has two parallel at a distance constrained by the two dimensions (2.00 and 1.00). After the sketch is constrained and dimensioned, select the Finish button to insert the hole feature. If you define more than one sketch point, you can insert additional holes at each point.

Hole Series
You can use the Hole Series option in the Hole wizard within an assembly to define holes that go through multiple parts. This feature creates in-context references among selected components. The Hole Series also lets you add Smart Fasteners to created holes. The example in Figure 1 shows a set of holes created with the Hole Wizard and Hole Series with the addition of a screw, top stack (washer), and bottom stack (washer and nut) that were defined based on the selections. Any changes made to the defined values update the holes and fasteners.

Hole Series dialog box.

Figure 5. Hole Series dialog box.

The Hole Series is an option when an assembly is active. Its tab appears at the end of the tab list within the Hole Wizard. Figure 5 shows the Hole Series dialog box, in which you can make separate settings for the top part, middle parts, and last part to define characteristics for the top hole and the clearance holes (middle parts and last part).

Hole Placement dialog box.

Figure 6. Hole Placement dialog box in Hole Series option.

The final dialog box is similar to the regular Hole wizard hole placement function, with the exception of the Add Smart Fastener option shown in figure 6. By selecting this option, you can define the top and bottom stack to add washers and nuts to the created hole(s). A limitation of the Hole Series feature is that when multiple instances of the same feature appear in an assembly, each instance must use a separate configuration to define the additional hole series.

The Hole Truth
The Hole wizard and its Hole Series option can save you time when adding holes to parts or an assembly. They help eliminate the need for reference books and charts to create properly sized holes for the desired fasteners. You can use Smart Fasteners to populate these holes either through the Hole Series option or by starting the Smart Fasteners function within the assembly and then selecting the desired holes. The Smart Fasteners feature determines the appropriate fastener type and lets you define the top and bottom stack.


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