How To Make a Threaded Hole With Hole Wizard in SOLIDWORKS

The Hole Wizard in SOLIDWORKS is the main tool for creating standard holes and tapped (threaded) holes without having to calculate drill sizes or sketch every hole from scratch. You choose a hole standard, type, size, and end condition, and SOLIDWORKS builds the correct hole geometry for you, including options such as counterbores, countersinks, straight taps, tapered taps, and slots.

Once a tapped hole is defined with Hole Wizard, you can either:

• Leave it as a cosmetic thread (recommended for performance and most production models), or
• Add detailed 3D thread geometry using the Thread feature for visual realism, 3D printing, or close-fit checks.

In this tutorial, you will model a simple rectangular block and add threaded holes using Hole Wizard and the Thread feature in SOLIDWORKS. The steps apply to recent versions of SOLIDWORKS (2016 and later, when the Thread tool was introduced), although the interface may differ slightly between releases.

What You’ll Need Before You Start

• SOLIDWORKS version: 2016 or newer is recommended if you want to use the Thread feature directly. Earlier versions can still create tapped holes with Hole Wizard but require a manual swept-cut method for physical thread geometry.
• Document units: Millimeters (mm) for this example.
• Basic skills: Familiarity with sketches, dimensions, planes, and simple features like Extruded Boss/Base and Extruded Cut.

Understanding Hole Wizard and Threads in SOLIDWORKS

Before jumping into the model, it helps to understand how SOLIDWORKS treats threaded holes:

• Hole Wizard: Defines the hole type (e.g., Straight Tap), the thread standard (ANSI Metric, ISO, etc.), size (e.g., M8 × 1.25), and end condition (e.g., Through All). It automatically picks the correct tap (minor) diameter for the selected thread.
• Cosmetic Threads: A lightweight visual representation of threads attached to the hole edge. They display correctly in drawings with thread callouts and are ideal for most engineering workflows because they don’t add heavy geometry.
• Thread Feature: Creates real 3D helical thread geometry on cylindrical faces. This is more detailed but also heavier on performance, so it’s best used selectively (for example on parts you intend to 3D print or render up close).

In this example, you will first define tapped holes with Hole Wizard and then generate physical threads with the Thread feature on those holes.

Step-by-Step: Creating a Threaded Hole With Hole Wizard

Step 1: Create the base block

1. Start a new part and set the units to millimeters (MMGS).
2. On the Top Plane, create a new sketch.
3. Sketch a rectangle and dimension it to 70 mm in length and 50 mm in width using Smart Dimension.
4. Exit the sketch and use Features > Extruded Boss/Base to extrude the rectangle to a thickness of 10 mm. This forms a simple cuboid as your base part.

Your model should look similar to the one shown below:

Step 2: Open Hole Wizard and choose a tapped hole type

1. Go to the Features tab on the CommandManager.
2. Click Hole Wizard. The Hole Wizard PropertyManager will appear on the left.
3. The PropertyManager has two key tabs:

• Type – controls the hole standard (e.g., ANSI Metric), hole type (e.g., Straight Tap), size, fit, and end condition.
• Positions – controls where the hole centers are placed on the selected face.

4. Under the Type tab, choose a hole standard such as ANSI Metric or ISO (depending on your template).
5. Under Hole Type, select Straight Tap (the icon circled in red in the original image). This tells SOLIDWORKS that you are creating a threaded (tapped) hole rather than a simple drilled hole.

For now, you can leave the default size and depth settings; you’ll refine them after placing the holes.

Step 3: Place the hole centers on the top face

1. Switch to the Positions tab of the Hole Wizard PropertyManager.
2. Click on the top face of the cuboid. SOLIDWORKS will usually reorient the model to the Top view automatically. If not, press the spacebar and choose Top from the Orientation dialog.
3. Move your cursor over the top face. You’ll see yellow previews of the hole center points following your cursor.
4. Left-click four times to place four hole centers roughly near the corners of the block. Don’t worry about exact locations yet; you will fully define them with dimensions.

To properly constrain the pattern:

• Add horizontal and vertical relations so that opposite hole centers are aligned.
• Use Smart Dimension to dimension each center from the edges (or from centerlines) so that all four holes are symmetrical about the midplanes of the block.
• Optionally, sketch construction centerlines across the rectangle (midpoint-to-midpoint) and make the hole centers symmetric about those lines for a fully defined, robust layout.

When you’re done, all hole centers should be fully defined and symmetrically placed, similar to the figure below:

Step 4: Define the tapped hole size and end condition

1. Once the positions are defined, click the green checkmark to exit the sketch portion, then immediately edit the Hole Wizard feature again (or stay in the PropertyManager if you didn’t exit).
2. Return to the Type tab in the Hole Wizard PropertyManager.
3. Under your chosen standard (e.g., ANSI Metric), set the hole specification:

• Hole Type: Straight Tap
• Size: For example, choose M8 × 1.25 (nominal diameter 8 mm, thread pitch 1.25 mm).
• End Condition: Set to Through All so the hole cuts completely through the 10 mm block.

You can also adjust other parameters if needed (thread depth, drill tip angle, etc.) depending on your design requirements. For a basic tutorial part, the defaults are usually sufficient.

At this point, you have four tapped holes defined by Hole Wizard. In most production models and drawings, you could stop here and rely on cosmetic threads and automatic hole callouts. In the next steps, you’ll go further and create physical thread geometry using the Thread feature.

Step 5: Access the Thread feature

The Thread feature lives in the same fly-out as Hole Wizard on the Features tab.

1. On the Features tab, click the small dropdown arrow under Hole Wizard to expand the fly-out menu.
2. Select Thread (circled red in the image). This opens the Thread PropertyManager.

If your version of SOLIDWORKS does not show the Thread command, you may be on a pre-2016 version, in which case you’ll need the older helix + swept cut method instead of the Thread feature.

Step 6: Configure the Thread feature on the tapped hole

The Thread PropertyManager lets you control how the physical thread is created: where it starts, how far it extends, which standard it follows, and whether it is modeled as a cut or an extrusion.

1. In the graphics area, click the circular edge at the opening of one of the tapped holes on the top face. This defines the Thread Location – the edge where the thread begins.
2. In the Thread PropertyManager, under Specification, set:

• Type: Metric Tap (for an internal, female thread).
• Size: M8 × 1.25 to match the Hole Wizard tapped hole size.

3. Under Thread Method, choose:

• Cut thread if you want the thread represented as removed material (typical for an internal threaded hole), or
• Extrude thread if you want the thread represented as added material (more common for external threads, such as on a bolt).

For an internal hole, Cut thread is usually more realistic, but you can use Extrude thread as in the original example if you are primarily interested in visual appearance and not using the feature for precise manufacturing dimensions.

4. Set the End Condition for the thread – for example:

• Up to selection (select the bottom face of the hole), or
• Blind with a depth slightly less than the thickness if you want a partially threaded hole.

5. Adjust advanced fields such as:

• Offset (to start the thread slightly below a chamfered edge),
• Right-hand or left-hand thread direction, and
• Pitch (if you are defining a custom thread).

6. When you are satisfied with the preview (it can help to enable a shaded preview if available), click the green checkmark to create the thread feature.

You should now see a helical thread modeled on the inside surface of the hole, as in the figure below:

Repeat the process for the remaining three holes, or use patterns if appropriate (for example, by threading one hole and then using a circular or linear pattern of the Thread feature, provided the geometry is patterned consistently).

Step 7: Use Section View to inspect the threaded holes

The thread geometry can be hard to see clearly from the outside of the block. A section cut gives you a much better view of the internal threads.

1. On the View toolbar or the Heads-up View toolbar, click Section View.
2. Choose a plane (for example, the Front Plane or a mid-plane) that cuts through the holes.
3. Adjust the section depth as needed to pass through the center of the threaded region.
4. Apply the section and rotate the model if necessary to confirm that:

• The hole goes all the way through (for “Through All” end conditions).
• The thread covers the intended depth along the hole wall.
• There are no unexpected gaps, collisions, or missing portions of the threads.

The sectioned model should resemble the illustration below:

Best Practices for Threaded Holes in SOLIDWORKS

• Use cosmetic threads for most parts: Physical threads add a lot of faces and can significantly slow large assemblies. In many workflows, cosmetic threads plus correct hole callouts on drawings are sufficient.
• Match Hole Wizard and Thread feature settings: Make sure the thread size and standard selected in the Thread feature match the tapped hole defined in Hole Wizard (for example, both as M8 × 1.25).
• Use standards-based sizes: When possible, stick to standard metric or Unified thread sizes so that tap drill diameters and callouts are correct and compatible with standard tooling.
• Model detailed threads only where needed: For 3D printing, rendered visuals, or interference checks in tight spaces, model physical threads on just a few critical components or configurations.
• Check the model with a section view: Always verify the depth, orientation, and coverage of the thread using Section View before relying on it in downstream steps like 3D printing or analysis.

Summary

By combining the Hole Wizard and Thread features in SOLIDWORKS, you can quickly create standard-compliant tapped holes and, when necessary, detailed 3D thread geometry. The Hole Wizard handles the correct drill size, thread designation, and positioning, while the Thread tool adds realistic helical geometry that can be inspected in section, rendered, or used in 3D printing workflows.

Once you are comfortable with the basic workflow in this simple 70 × 50 × 10 mm block, you can apply the same process to real components such as brackets, housings, manifolds, and custom fixtures, using different standards, sizes, and patterns of threaded holes.