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# How to make threads in SOLIDWORKS, cosmetic or modeled
- URL: https://www.solidsworks.com/threads-in-solidworks/
- Published: 2026-11-03T13:32:29.000Z
- Updated: 2026-11-03T13:32:29.000Z
- Description: Cosmetic threads for drawing callouts, modeled geometry for printing and close views. A shaft-and-hole workflow with drawing import and interference checks.
- Author: David Foster
- Tags: Parts and features

In SOLIDWORKS Design 2026, use **Insert > Annotations > Cosmetic Thread** on the starting circular edge when the thread needs a drawing callout. For a thread that needs helical faces in the model, use **Insert > Features > Thread**. I'd choose cosmetic threads for ordinary machined holes and stock fasteners because they keep the thread specification attached to the feature without building the helix. A thread that goes to a printer needs actual geometry.

## Choose what the file must contain

A [cosmetic thread stores thread attributes](https://help.solidworks.com/2026/english/SolidWorks/sldworks/c%5Fcosmetic%5Fthreads.htm?ref=solidsworks.com) on an existing feature. It represents the minor diameter on a boss or the major diameter in a hole and can carry a drawing callout. The underlying solid still has a plain cylindrical surface. A modeled thread adds a swept cut or boss, so its grooves or ridges become part of the solid.

| Deliverable                                        | Choose                                                               | What to check                                                |
| -------------------------------------------------- | -------------------------------------------------------------------- | ------------------------------------------------------------ |
| A drawing for a tapped hole or threaded shaft      | Cosmetic Thread, or a Hole Wizard tapped hole with a cosmetic thread | Standard, size, depth and drawing callout.                   |
| An ordinary assembly using stock screws            | Cosmetic threads unless the helical shape is required                | Matching specifications, alignment and interference results. |
| A close view whose silhouette must show the thread | Modeled Thread                                                       | Profile, pitch, handedness and end treatment.                |
| A printed part with working thread surfaces        | Modeled Thread with a profile adapted to the job                     | Mating geometry and the printer/material process.            |

Cosmetic threads avoid the extra helical faces that a modeled feature creates. Keep that lighter representation for routine assemblies and drawings; add the geometry when the deliverable needs its shape.

[![A smooth shaft with a thread callout beside a shaft with helical thread faces.](https://storage.ghost.io/c/4c/fc/4cfc073a-f190-4bcc-b2ab-759be23dfa61/content/images/2026/11/a09-thread-representations-ffaa39828fa2.webp)](https://storage.ghost.io/c/4c/fc/4cfc073a-f190-4bcc-b2ab-759be23dfa61/content/images/2026/11/a09-thread-representations-ffaa39828fa2.webp?ref=solidsworks.com)

A cosmetic thread carries the specification on a plain solid. A modeled thread puts the helical faces into the solid.

## Add a cosmetic thread to a shaft or hole

Start with the cylindrical boss or hole already present. Cosmetic threads work on internal and external features; you don't need a modeled helix to identify a tapped hole.

[![Circular starting edges highlighted on a plain cylindrical boss and the entrance of a cylindrical bore.](https://storage.ghost.io/c/4c/fc/4cfc073a-f190-4bcc-b2ab-759be23dfa61/content/images/2026/11/a09-starting-circular-edge-fe88fc373525.webp)](https://storage.ghost.io/c/4c/fc/4cfc073a-f190-4bcc-b2ab-759be23dfa61/content/images/2026/11/a09-starting-circular-edge-fe88fc373525.webp?ref=solidsworks.com)

Choose the circular edge where the thread begins; the cylindrical face and the flat end face are different references.

1. Select the circular edge where the thread starts. On a cylindrical shaft or hole, this is the rim of the threaded region.
2. Click **Insert > Annotations > Cosmetic Thread**, or use **Cosmetic Thread** on the Annotation toolbar.
3. Under **Thread Settings**, choose **Standard**, **Type** and **Size**. The Size list contains valid values for the selected edge.
4. Set **End Condition**: **Blind** for a specified depth, **Through** through the existing geometry, or **Up to Next** to the next intercepting entity. Enter **Depth** for Blind.
5. Check the thread callout and confirm the feature. When a standard drives the callout, its text cannot be edited directly in this PropertyManager.

The [edge-selection rule changes for conical features](https://help.solidworks.com/2026/english/SolidWorks/sldworks/t%5Finsert%5Fcosmetic%5Fthreads.htm?ref=solidsworks.com): select the major diameter of a conical hole or the minor diameter of a conical boss. The [Cosmetic Threads PropertyManager](https://help.solidworks.com/2026/english/SolidWorks/sldworks/HIDD%5FDVE%5FCTHREAD.htm?ref=solidsworks.com) then exposes the applicable diameter or conical offset.

If you want shaded thread markings on the model, open **Tools > Options > Document Properties > Detailing** and select **Shaded cosmetic threads** under **Display filter**. This changes the display; it doesn't cut grooves into the solid. Also check that the parent feature or component is visible, because cosmetic-thread visibility follows its parent.

### Use Hole Wizard for a new tapped hole

For a new standard tapped hole, I'd start with **Hole Wizard** because the hole type, size and annotation stay in one feature. Select a face, click **Insert > Features > Hole Wizard**, choose **Straight Tap** or **Tapered Tap**, then set the standard, type, size and end condition. Use the Positions tab to locate the hole.

In the [Hole Wizard thread options](https://help.solidworks.com/2026/english/SolidWorks/sldworks/r%5FHIDD%5FDVE%5FHW%5FHOLE%5FSPEC.htm?ref=solidsworks.com), **Cosmetic thread** cuts the bore at the tap-drill diameter and adds the thread representation. **With thread callout** adds its drawing annotation. Neither option creates helical faces. For a blind tapped hole, the tap thread depth cannot exceed the blind hole depth.

## Show the thread on the drawing

Cosmetic threads from part documents enter drawing views automatically. Callout behavior follows the drawing standard: ANSI drawings insert thread callouts automatically; ISO, JIS and other standards don't use that same automatic callout behavior. If a defined callout is missing, right-click the cosmetic thread in the drawing and choose **Insert Callout**.

Assembly drawings need an import check. Use **Insert > Model Items** and select **Cosmetic thread**, or enable **Cosmetic Threads - assembly (may affect performance)** under **Tools > Options > Document Properties > Detailing > Auto insert on view creation**. In the Drawing View PropertyManager, check **Import annotations** and **Cosmetic threads** under Import options. These are the documented [assembly-to-drawing import controls](https://help.solidworks.com/2026/english/SolidWorks/sldworks/c%5Fcosmetic%5Fthreads.htm?ref=solidsworks.com).

For a Hole Wizard hole, use **Insert > Annotations > Hole Callout**, select the hole edge and place the note. The [Hole Callout reads the hole information](https://help.solidworks.com/2026/english/SolidWorks/sldworks/t%5Fadding%5Fhole%5Fcallouts%5Fdrawing.htm?ref=solidsworks.com), including additional Hole Wizard data. Keep its size and type variables instead of replacing the whole note with typed text.

## Model an external thread with the Thread feature

Start with a cylindrical shaft whose diameter comes from the intended thread design. SOLIDWORKS states that [Thread does not autosize to the model](https://help.solidworks.com/2026/english/SolidWorks/sldworks/r%5Fthread%5Fpropertymanager.htm?ref=solidsworks.com). Selecting a shaft edge does not select a compatible thread size for you.

1. Select the starting circular edge and click **Insert > Features > Thread**.
2. Under **Thread Location**, check **Edge of Cylinder**. Set a start offset only if the thread must begin away from that edge; check its direction in the preview.
3. Under **Specification**, select the intended **Type** and **Size**. For the documented external cut-thread example, SOLIDWORKS uses Metric Die and M6x1.0; those are example selections, not values for every shaft.
4. Select **Cut Thread** to remove material with the profile, or **Extrude Thread** to add it. Inspect how the profile meets the shaft before accepting the method.
5. Set **End Condition**. Use **Blind** and Depth for a length, **Revolutions** for a turn count, or **Up to Selection** for a plane or planar face [perpendicular to the thread axis](https://help.solidworks.com/2026/english/SolidWorks/sldworks/r%5Fthread%5Fpropertymanager.htm?ref=solidsworks.com). Check the start and end of the preview.
6. Choose **Right-hand thread** or **Left-hand thread** under Thread Options. Inspect the complete preview and confirm.

[![Thread PropertyManager fragments with Type set to Metric Die, Size set to M6x1.0, and Cut thread selected.](https://storage.ghost.io/c/4c/fc/4cfc073a-f190-4bcc-b2ab-759be23dfa61/content/images/2026/11/a09-thread-profile-method-ff3935f16e04.webp)](https://storage.ghost.io/c/4c/fc/4cfc073a-f190-4bcc-b2ab-759be23dfa61/content/images/2026/11/a09-thread-profile-method-ff3935f16e04.webp?ref=solidsworks.com)

In this [external cut-thread example](https://help.solidworks.com/2026/english/SolidWorks/sldworks/t%5Fcreate%5Fcut%5Fthread.htm?ref=solidsworks.com), Type is Metric Die and Size is M6x1.0\. Cut thread removes material.

The [cut-thread example](https://help.solidworks.com/2026/english/SolidWorks/sldworks/t%5Fcreate%5Fcut%5Fthread.htm?ref=solidsworks.com) establishes the command and an example profile. Your shaft diameter, profile and thread length still have to agree. If you use **Trim with start face** or **Trim with end face**, the profile must extend beyond the trimming face.

The built-in Type and Size profiles are [nominal profiles that need modification for production-quality threads](https://help.solidworks.com/2026/english/SolidWorks/sldworks/r%5Fthread%5Fpropertymanager.htm?ref=solidsworks.com). Check the specified thread form, dimensions and tolerances before sending modeled geometry for fabrication.

### For an internal modeled thread, check the bore and profile together

Prepare the intended cylindrical bore, select its starting inner circular edge and open the same Thread command. Choose the profile and size for the internal thread, then inspect their position against the bore wall with **Locate Profile**. Set the thread method, end condition and handedness as above.

Cut Thread works when the selected profile removes the required material from that bore. Another profile and starting bore may require Extrude Thread to add the helical ridge. The [thread guidelines explicitly warn](https://help.solidworks.com/2026/english/SolidWorks/sldworks/r%5Fthread%5Fguidelines.htm?ref=solidsworks.com) that a cut profile which works on a shaft may require extrusion on a hole. There is no reliable rule that every internal thread must use Cut Thread.

[![A bore-wall section with a cut recess beside a section with an added ridge joined to the body; grey dashed lines mark the original wall.](https://storage.ghost.io/c/4c/fc/4cfc073a-f190-4bcc-b2ab-759be23dfa61/content/images/2026/11/a09-profile-body-cut-extrude-cf7049d34ae2.webp)](https://storage.ghost.io/c/4c/fc/4cfc073a-f190-4bcc-b2ab-759be23dfa61/content/images/2026/11/a09-profile-body-cut-extrude-cf7049d34ae2.webp?ref=solidsworks.com)

The grey dashed line marks the original bore wall. Cut Thread removes material from the body; Extrude Thread adds material into the bore while staying joined to the body. The profile and starting bore determine the method.

If the feature fails after changing an offset, restore the previous offset and try a smaller change. A profile displaced away from the underlying body can lose contact. Check diameter and pitch overrides too; a profile name alone doesn't establish the final thread geometry.

## Check the joint before treating it as a fit

For an assembly, open **Tools > Evaluate > Interference Detection** and select the components. Resolve the components for an accurate check: Large Design Review uses approximate calculations and omits some options.

Enable **Create matching cosmetic threads folder**, then click **Calculate** to separate interferences between components with properly matched cosmetic threads. Mismatched or misaligned threads and other interfering geometry remain in the ordinary results. **Create fasteners folder** is a separate grouping option; neither folder is a blanket instruction to ignore every screw-related clash. These distinctions are defined in the [Interference Detection options](https://help.solidworks.com/2026/english/SolidWorks/sldworks/HIDD%5FDVE%5FINTERFERENCE.htm?ref=solidsworks.com).

For a printed joint, inspect actual helical faces and the mating part, then check a sample made with the intended printer, material and settings. Cosmetic markings cannot supply missing geometry to the exported mesh. Choose any fit allowance for that process rather than copying an unexplained clearance.

## Change the design and follow the reference

Change one driving dimension deliberately, then rebuild. For a cosmetic thread, inspect the selected edge, thread size and depth, and reopen the drawing to check the callout. For a Hole Wizard tapped hole, changing Size updates its calculated depths only while **Automatically Calculate Depth** remains selected.

For a modeled thread, changing the shaft or bore diameter does not make Thread choose a new profile. Recheck Type, Size, any diameter or pitch overrides, the starting edge and the end condition. Inspect both ends and the mating component again. Continue with the appropriate [part-feature workflow](https://www.solidsworks.com/tag/parts-and-features/) only after the geometry and the drawing describe the same intended thread.