Parametric Threads in SolidWorks

It is possible with SolidWorks to model two pieces mated with metric threads, and have completely parametric drawings. The system partially works with UN threads, and will not work with ACME or Whitworth threads.

How it works

A metric screw thread is cut to a 60° angle. If this angle is drawn sharp, the face on either side of the thread will equal the thread pitch. This makes for a thread modeled with a height of .866×pitch. A real metric thread has a height of 5/8×pitch.

This means that your minor diameter is modeled slightly smaller than a real one. This is good. Any features that appear to be close to your minor diameter actually are not that close.

How to do it

  1. Model of female thread Sketch and revolve the outside threaded housing. Note how the dimensions are applied. It does not matter whether you start with the outside or inside thread. The thread size is the major, outside diameter. The thread is shown with a pitch of 2mm. The solid and the sketch lines angled 60° apart are modeled equal in length, making an equilateral triangle.
  2. I like to model the undercut at the flange end of the thread parallel to the sketch line, and equal in length to the side of the thread. This makes it equal to the pitch. You can do this part any way you darn well please.
  3. Female thread with model dimensions Create the drawing views and apply dimensions. You can use SolidWorks' reference dimension feature, or you can insert model items so that the model parametric dimensions are applied.
  4. Female thead with thread dimensions Clean up and organize the dimensions.
  5. Attach a note to the outside of the thead. Type "M", click on 44, type "X", then click on the 2mm dimension. Probably, you will have to edit the 44mm dimension to remove the diameter symbol.
  6. I added a sketch line to represent the major diameter of the thread. I modified line thicknesses and styles to make the drawing conform as much as possible drafting standards.
  7. Complete drawing of female thread Hide the two thread dimensions.
  8. Fix your tolerances (I did not bother here), and this drawing is done.
  9. Create an assembly and attach your part to it.
  10. Exploded assembly model Create your male threaded part, and attach it to your assembly, as shown. I have turned on SolidWorks' section view. I have not mated the faces yet.
  11. Mate the faces.
  12. Sketch of outside housing Flip on the sketch of the outside housing.
  13. Use the the geometry of the outside housing to control the major and minor diameters of the male thread. You can control the tooth angles as well, but this whole technique only works if it is 60°.
  14. Flip off the sketch of the outside housing.
  15. Assembly drawing Here is the resulting assembly drawing.
  16. Drawing with visible dimensions Create the drawing of your male thread and apply reference dimensions as shown. Model dimensions do not work because you have not applied the required dimensions to your model. Since the thread profile is an equilateral triangle, the diagonal side is equal to the pitch. This techique would work on Unified National threads if you could convert your pitch to threads per inch. It will not work on Whitworth or ACME threads. Apply the thread note as described above.
  17. Reference dimensions hidden Hide your two reference dimensions.
  18. Apply the other dimensions and tolerances. I did not bother here.
  19. Modified drawing Move to your assembly drawing. On the outside housing, change the thread pitch from 2mm to 1mm. Alternately or in addition, you can change the thread major diameter.
  20. Load the outside housing drawing and note how the scale drawing and the thread specification have updated correctly.
  21. Load the male thread drawing and now how its sketch and thread specification have updated correctly.

Final Remarks

This is a modeling and design technique. Finalizing models with parametrically controlled features, and checking them into PDM is a bad idea. If someone checks out the outside housing and modifies the thread, you can load the assembly and it will appear that the inside thread is good too. Traditional design change rules of not changing form, fit and function continue to be good policy.

This is a process for making a drawing you can send to a machine shop that will work from your drawings. If you want to rapid prototype if your model, you can going to have to model your threads correctly, and perfectly.

When you are finished with your design, load the assembly, edit the inside thread, and replace the parametric geometry controls with local dimensions.

Last modified: 2010May29 Howard Gibson