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Project 4

How to model a bottle with a thread in SOLIDWORKS

A bottle combines three techniques: a revolve for the body, a shell for the wall and a thread on the neck. Since SOLIDWORKS 2016 the Thread feature can add the neck thread directly, and Bottle is one of its built-in profile types. The manual alternative — a helix and a sweep — still teaches the most and works in every version.

Kevin Walsh Kevin Walsh Updated Checked for SOLIDWORKS 2026
3D render of the bottle with a threaded neck from the SOLID WORKS Club project
Level
Project
Time
40 min
Material
Plastic (any)

Specification

Parameter Value
Body diameter / height Ø70 / 150 mm
Shoulder R21 arc to the neck
Neck diameter / height Ø28 / 19 mm
Wall thickness 1.5 mm (shell, open top)
Thread Pitch 4 mm, 2 turns, starting 5 mm below the rim

The drawing

Dimensioned drawing of the bottle with a threaded neck project with orthographic and isometric views
Dimensions in mm, third-angle projection. Download the PDF to print it.

Step by step

1. Revolve the body

Front plane: centreline, half profile up to the shoulder, an R21 arc to the neck, neck to 190 mm. Revolve 360°.

2. Shell

Shell 1.5 mm and remove the top face of the neck.

3. Thread with the Thread feature

Insert → Features → Thread, pick the neck's top edge as the start, add an offset, choose the Bottle type, set pitch and turns, and make it an extruded (not cut) thread.

4. Or sweep along a helix

Helix on the neck circle: pitch 4, 2 turns. Sweep a small trapezoid profile along it without merging, cap or trim both thread ends, then combine the bodies.

5. Finish

Fillet the thread ends and the base edge. For drawings, consider a simplified configuration without the thread — physical threads are the slowest features to rebuild.

Check your result

  • Overall height 190 mm, body Ø70, neck Ø28.
  • Our STEP model (body plus swept thread) has a volume of 64,660.09 mm³.

Compare your model with the STEP file above — it opens in SOLIDWORKS and most other CAD programs.

Next: project 5 — m10 bolt and nut.

Download files

Commands used

Show solution
  1. Revolve the body. Front plane: centreline, half profile up to the shoulder, an R21 arc to the neck, neck to 190 mm. Revolve 360°.
  2. Shell. Shell 1.5 mm and remove the top face of the neck.
  3. Thread with the Thread feature. Insert → Features → Thread, pick the neck's top edge as the start, add an offset, choose the Bottle type, set pitch and turns, and make it an extruded (not cut) thread.
  4. Or sweep along a helix. Helix on the neck circle: pitch 4, 2 turns. Sweep a small trapezoid profile along it without merging, cap or trim both thread ends, then combine the bodies.
  5. Finish. Fillet the thread ends and the base edge. For drawings, consider a simplified configuration without the thread — physical threads are the slowest features to rebuild.

Sources

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

Frequently asked questions

Does SOLIDWORKS have a bottle thread profile?

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Yes. The Thread feature ships with Die, Tap and Bottle profile types in several sizes; copy one to make a custom profile.

Why are threaded models slow?

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Physical threads are heavy geometry. In one test the Thread feature took about 96% of a part's rebuild time; use cosmetic threads or a simplified configuration where you can.