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
-
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.
-
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.
-
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.
-
Clean up and organize the dimensions.
-
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.
-
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.
-
Hide the two thread dimensions.
-
Fix your tolerances (I did not bother here), and this drawing is done.
-
Create an assembly and attach your part to it.
-
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.
-
Mate the faces.
-
Flip on the sketch of the outside housing.
-
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°.
-
Flip off the sketch of the outside housing.
-
Here is the resulting assembly drawing.
-
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.
-
Hide your two reference dimensions.
-
Apply the other dimensions and tolerances. I did not bother here.
-
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.
-
Load the outside housing drawing and note how the scale drawing and
the thread specification have updated correctly.
-
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.
PS
It is possible to model Unified National, Whitworth, ACME
and various other non-metric threads.
It is a bit more complicated.
Use the equation editor.
Within the equation editor, specify the threads-per-inch.
Convert this to pitch for your model.
Add the TPI to your list of properties.
If you are using fractions or screw numbers,
set these up as properties too.
This can be used to work around millimetre/inch conversions.
In your drawing on the dimension note, call up the property.