Creating NPT threads in SOLIDWORKS

Article by TriMech Solutions, LLC updated September 28, 2022


The Hole Wizard has callouts to be able to identify NPT threads in SOLIDWORKS, but what about when you need to model the thread? The following tutorial will walk you through creating an NPT thread, this example consists of a ½” NPT thread. For the values found here, and for other NPT sizes, please refer to the National Standard Taper Pipe Threads Size NPT Chart.

To begin, create the cylindrical base for the threads using the nominal value of the NPT thread size desired, in the case of a ½” NPT thread, the outside diameter of the base is 0.840”.

  1. Apply the standard taper rate to the base. Do this by sketching the contour highlighted in orange and making the angle between the two noted lines the standard 1.7899°. Once the sketch is complete, perform a revolve cut using this contour.

apply standard taper rate

  1. Create the path for the threads using the Helix and Spiral command. Select a plane, face, or edge to sketch a circle to define the cross-section of the helix. Choose the flat face of the base and Convert Entities or sketch a circle to match the outside diameter.

helix and spiral command

Once the sketch is finished the Helix/Spiral PropertyManager automatically opens. Define the Helix/Spiral by Pitch and Revolution, a ½” NPT thread has a pitch of 14, so in the Pitch box enter 1/14” (0.07142857”). Reverse the direction if necessary to have the threads run along the base and set the number of revolutions desired. Enable Taper Helix and set the taper angle to match the standard taper used earlier (1.7899°). Enable Taper outward. Click the green checkmark to exit the command.

define helix spiral


  1. Create the “tool” to make the cut. Sketch a reference line along the center of the base and sketch a triangle using reference lines as shown, make the two sides of the triangle bounded by the 60° angle equal and insert a point at the midpoint of one of the equal sides, this point will define the pitch diameter.

create tool to make the cut

Set the distance between the reference line along the center of the base and the midway point on the triangle equal to half the pitch diameter, found to be 0.379215 for a ½” NPT thread. Create the closed contour of the cutting tool by tracing the triangle’s reference lines as seen below leaving a small section for the root. Dimension the height of thread using the value obtained from the NPT thread table, here it is 0.05714. The root is always pitch divided by 8 for external threads, in this case it is 1/14 divided by 8, equaling 0.00893.

  1. Create the threads using the Swept Cut command. Select the triangular cutting tool as the profile and the Helix/Spiral as the path.
  2. For a cleaner finish highlight the face shown below and select Convert Entities, cut extrude through the base.

creating NPT threads: convert entities

It should look like this:

final NPT thread

Related Links

Certified SOLIDWORKS Services available from Javelin

Javelin can help you to:

Find Related Content by TAG:

TriMech Solutions, LLC

TriMech provides thousands of engineering teams with 3D design and rapid prototyping solutions that work hand-in-hand, from sketch to manufacturing. Javelin became a subsidiary of TriMech Solutions LLC in 2021.