Using the Stud Wizard in SOLIDWORKS 2022

Historically, SOLIDWORKS users have been somewhat limited with respect to available approaches for representing external threads in part and assembly designs. Though thread callout annotations and graphical representations (cosmetic threads) are still very commonly used due to their simplicity in both models and drawings, they typically do not represent the true manufactured form of a design. Only if the additional features to accurately represent threads are added can we be sure to avoid downstream problems in assemblies where component fit and interference are critical.

In the image below (left), we see a common scenario where a cosmetic thread has been applied to a cylinder of a diameter larger than the thread itself. Though this may be acceptable by some drafting standards for manufacturing, it may result in difficulties at the assembly level. To solve this, the excess material would need to be cut away prior to applying the cosmetic thread (right), which may require multiple features if the threads do not extend up to next or through.

The release of the Thread feature in 2016 offered designers a simplified approach to creating helical thread geometry for a more accurate and realistic representation of threads, but it still left a bit to be desired. The Thread feature, while extremely powerful, was also rather complex and resulted in significantly slower rebuild times when applied frequently. Additionally, automatic callouts are not supported for Thread features, making it more difficult to communicate through manufacturing drawings. Because of this, the Thread command is typically reserved for modeling non-standard threads which cannot otherwise be communicated.

SOLIDWORKS 2022 introduces the Stud Wizard, a brand-new feature specifically designed to split the difference between overly-simplistic thread callouts/cosmetic threads and the slow, complex accuracy of the Thread feature. As the name implies, the Stud Wizard functions very similarly to the Hole Wizard and is specifically geared toward creating externally-threaded studs to complement the existing capability of the Hole Wizard for internally-threaded holes.

By default, the Stud Wizard command can be found in the Features tab of the CommandManager by clicking the dropdown arrow underneath the Hole Wizard.

Creating a Stud on an Existing Cylinder

Once activated, the Stud Wizard provides two different modes to choose from to create a stud, which can be toggled using the icons at the top of the PropertyManager.

The first mode allows the use of an existing cylindrical body, similar to what would be required to use a Thread or cosmetic Thread feature. Simply select the outside circular edge of the existing stud body, then specify the standard, type (machine threads or straight pipe tapped thread) and size as you would for a Hole Wizard. It should be noted that just like the Hole Wizard, available standards for the Stud Wizard are controlled by the Toolbox Configuration properties. Additionally, when creating a stud from an existing cylinder body, available sizes are limited by the diameter of the cylinder. In this case, since the cylinder diameter is 5/8”, the available sizes are 9/16” and smaller.

Thread depth can be controlled using a Blind end condition with a depth value (1” in this example), Up to Next, or Through for added flexibility. Additionally, thread class options can be enabled to communicate a tolerance of 1A, 2A or 3A. For the uninitiated, the “A” in this designation indicates that the threads are external (internal thread are designated with the letter B), while the numeric value represents the closeness of the fit. Generally, a higher-class number indicates a tighter fit, with class 2A being the most common due to its balance of manufacturing difficulty/cost and performance.

It should be noted that specifying a thread class in the Stud Wizard feature will not change the nominal dimensions of the stud, nor will it apply any type of tolerance; however, if a thread callout is inserted for the feature, it will include the thread class designation if one was applied.

Finally, the undercut checkbox may be enabled to cut away material below the threads for proper assembly and fit of components. Simply specify a diameter for the undercut (limited to a maximum equal to the thread diameter), a depth value and a fillet radius to be applied to the edges of the undercut. Note that if a blind end condition is in use for the stud, the undercut depth is limited to the remaining space between the end of the threads and the end of the cylinder body.

Once the Stud Wizard feature is completed, a thread callout annotation can be inserted by expanding the stud feature in the design tree, right clicking the Stud Thread sub-feature and selecting Insert Callout from the shortcut menu. Alternatively, callouts may be added by right clicking the graphic circle representing the Stud Thread feature (if visible). Note that the visibility of cosmetic threads is controlled by the “View Top Level Annotations” setting in the Hide/Show Items dropdown menu, which must be enabled to see them. Thread callouts may also be inserted into drawing views.

As seen here, the Stud Wizard feature allows you to quickly define externally threaded studs using familiar standards while representing the intended geometry more accurately and avoiding the complexity (and documentation difficulty) associated with full helical threads. Though using the Stud Wizard on an existing cylinder is certainly efficient on its own, the second available mode allows you to create a stud entirely from scratch in a fashion almost identical to that of the Hole Wizard.

Creating a Stud on a Surface

Begin by activating the Stud Wizard feature as you would normally, then select the second icon labeled “Creates Stud on a Surface.” Once this mode is activated, two tabs become available in the PropertyManager.

The Stud tab provides all the same fields for defining thread parameters as seen in the first mode above, but also includes an additional Shaft Details section where the shaft length and diameter must be defined as this mode creates a brand new stud rather than using an existing cylinder feature. Also like the first mode, the available thread sizes are limited by the diameter value applied in the shaft details section.

Once shaft details and thread standards have been defined, the Position tab can be used to locate the new stud in a manner nearly identical to that of the Hole Wizard. However, as of this release, there are several limitations for the positioning of new studs. Unlike the Hole Wizard, selection of reference planes and non-planar faces is not currently supported as of this release; only planar faces are supported.

Additionally, though a sketch point is used to position the center of the stud, all other sketch tools including the Smart Dimension tool are unavailable while placing the point. If construction geometry or dimensions are required for position, the resulting point sketch must be edited after the stud feature is completed. Finally, multiple sketch points are not currently supported, meaning that each stud requires its own unique feature. Alternatively, mirror/pattern features may be used, but the Insert Callout command will not be available for the threads of the mirrored instances.

There also appears to be a potentially frustrating bug when using this mode. If the Through or Up to Next end condition is selected for the threads, the diameter field in the Shaft Details section becomes uneditable. Normally this would not be an issue, as the thread diameter would take priority and allow the stud to size properly; however, the diameter value in the shaft field still limits the available sizes in the thread standard section (illustrated below).

To solve this, temporarily set the end condition for the threads to Blind so that the shaft diameter field becomes editable once again, then set the shaft diameter to a value larger than the threads you would like to use. You’ll then return to the original end condition and the larger sizes should be available.


The Stud Wizard is a welcome new feature for SOLIDWORKS 2022 that takes advantages of the familiar Hole Wizard workflow to make externally threaded studs easier than ever before while balancing model accuracy with complexity and performance. The resulting model geometry is more accurate (and requires less work) than traditional cosmetic threads while avoiding the slow rebuild times associated with geometrically accurate helical thread features. While there are a few existing limitations to Stud Wizard as of the current release, they’re certainly not showstoppers. We expect to see additional improvements that will make the Stud Wizard even more useful.

Learn more about the new enhancements to SOLIDWORKS 2022 in the ebook SOLIDWORKS 2022 Enhancements to Streamline and Accelerate Your Entire Product Development Process.

About the Author

Jacob Ames is a Senior SOLIDWORKS Applications Engineer with Hawk Ridge Systems based out of Olympia, WA. He’s been producing SOLIDWORKS content, training students, and providing product demonstrations for over 5 of his 10+ years of CAD experience. If he’s not in front of his computer, you’ll likely find him playing video games or wandering the trails of the Pacific Northwest.

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