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Features · Lesson 13

SOLIDWORKS Thread feature

The Thread feature, added in SOLIDWORKS 2016, models real helical threads on shafts and holes from a library of profiles. Use it when the thread geometry itself matters — 3D-printed parts, realistic renderings, or threads that are not standard. It is much faster to set up than a helix and sweep, but modelled threads are heavy, so keep them out of big assemblies or suppress them in a simplified configuration.

Kevin Walsh Kevin Walsh Updated Checked for SOLIDWORKS 2026
3D printed bolt and nut with modelled helical threads next to the CAD model

Where to find it

Insert → Features → Thread (also in the Hole Wizard flyout)

Thread feature options

Option What it does
Edge / start location Where the thread starts; an offset can move it
Type and size Profile library: die (external) or tap (internal), inch or metric
Cut / Extrude thread Removes material from a shaft, or adds thread material
End condition Thread length
Right / left hand Thread direction
Trim with start/end face (2017+) Ends the thread flush with the faces
Multiple starts (2017+) Multi-start threads

Before the Thread feature, threads were made with a helix and a sweep — still useful for unusual profiles, but slower: in a CATI test the Thread command rebuilt in about 2.3 s versus 7.25 s for a helical sweep.

Practise it: the neck of the threaded bottle and the M10 bolt and nut.

Step by step

  1. 1

    Make the shaft

    Extrude a Ø10 circle 30 mm — the shaft from the cosmetic thread lesson, without its cosmetic thread.

  2. 2

    Start the Thread feature

    Insert → Features → Thread. Pick the circular edge at the end of the shaft as the start location.

  3. 3

    Choose the profile

    Pick a metric die profile (dies cut external threads) and size M10. Choose Cut thread, set the end condition to the length you need, and keep right-hand threads unless you need left-hand.

    Thread PropertyManager with metric die M10 profile and cut thread on a shaft
    Pick the start edge, a die profile and size, and cut the thread.
  4. 4

    Clean up the ends

    Tick Trim with start face and Trim with end face (since 2017) so the thread ends flush instead of with a partial turn sticking out.

Common mistakes

  • Modelled threads on every fastener in an assembly. They dominate rebuild time — use cosmetic threads unless geometry is needed.
  • Tapered or conical faces — the Thread feature does not support them.
  • Printed threads with no clearance. Add a small offset; TriMech used about 0.3 mm for a printed cap.
  • Missing profile library after a reinstall. Point File Locations to the Thread Profiles folder.

Lesson 13 of 18 in the features course.

Practice

Add an M10 cut thread to the Ø10 × 30 mm shaft. Check: open Evaluate → Performance Evaluation — the Thread feature should be by far the slowest feature in the part. Suppress it and compare the rebuild time.

Sources

Checked November 2026. SOLID WORKS Club is independent; menu names can differ slightly between releases.

Frequently asked questions

How do I make a real thread in SOLIDWORKS?

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Use Insert → Features → Thread, pick the edge where it starts, choose a profile and size, and set the length. For external threads choose a die profile; for internal threads a tap profile.

Should I use modelled or cosmetic threads?

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Cosmetic for nearly everything — they are fast and give drawing callouts. Modelled threads for 3D printing, renderings and special threads.

Why is my part slow after adding a thread?

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Helical geometry is expensive to rebuild. In one reseller test the Thread feature took 96% of a part's rebuild time. Suppress it in a simplified configuration.

Where are the thread profiles stored?

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In C:\ProgramData\SOLIDWORKS\SOLIDWORKS 20xx\Thread Profiles, set in System Options → File Locations.