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How to create an external cut thread in SolidWorks?

Cosmetic threads are generally preferred over physically modeling each thread as they save time and are lightweight. However, as the name suggests they are purely cosmetic.  If modeling of the thread is critical to the design (e.g. design of a screw jack or turnbuckle) or the thread is to be machined, follow the instructions for either of the methods below to model the thread.

There are a few methods to create an external (male) thread on a cylindrical body.

Insert Thread Feature

The easiest method to create a thread feature is to insert a thread.  The following example will use an M10x1.0 thread. Look up the major diameter for the thread to be inserted and set the diameter of the cylindrical feature (shaft) to suit. An optional step is to include a 0.75mm chamfer to the end of the shaft.  Insert a thread to an existing cylindrical feature by selecting “Insert” – “Features” – “Thread…”, or expand the drop down from hole wizard from the features tab and choose thread.  The steps to create the threaded cut are as follows:

  1. Edge – Select the edge at the end of the shaft where the thread is to be placed.
  2. Offset mm – Set to 2mm flip direction, as required, such that the thread starts before the start of the shaft.  This will fade out the start of the thread as opposed to the thread abruptly ending.
  3. Offset Angular – use this option if the start of the thread needs to be in a specific location.  Set to 0° for this example.
  4. End condition/length – Blind/10mm.  Use blind/revolutions to set the threaded length in terms of mm or revs respectively.  Up to selection can be used to thread the entire length (e.g. up to the under side of a hexagonal head).
  5. Type – Metric Die (die for external/tap for internal threads).  Alternatively select the thread type desired.
  6. Size – M10x1.0, or select the size that is required.
  7. Thread method – Cut.
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Swept Cut

Custom Sketch

Should a custom thread or different thread standard be required, create the sketch and use a swept cut. The steps to create the threaded cut are as follows.

  1. Chamfer end to 0.75mm (optional).
  2. Create a plane offset by 1mm from the face where the thread will start.  Similar to the previous example, this will fade out the start of the thread.
  3. Create a sketch on the new plane and use convert entities to create the sketch entity of the shaft’s edge.
  4. Select the drop down from “Curves” on the CommandManager, select the helix option.  Edit the helix for a 1.0mm pitch or the pitch of the desired thread,  and set 20 revolutions as the length. Set the thread to be clockwise.
  5. Start a new sketch and create the thread profile. Consult the thread charts as required. Use the pierce constraint to constrain the sketch point to the helix.
  6. Use the swept cut feature from the CommandManager, select the sketched thread as the profile and the helix as the path.
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Follow the same procedure for threads of any type.

Die Library File

This method uses the library thread sketches from SolidWorks and the similar steps as in method 2. Insert the sketch for the thread from the SolidWorks Library file located in the following directory: “C:\ProgramData\SOLIDWORKS\SOLIDWORKS 20XX\Thread Profiles”.  If this folder location has been setup as part of the design library the same file can be accessed from the Task Pane.  In either case, drag and drop the file into the graphics area of the part that is being edited.  The steps for this method are as follows:

  1. Optional 0.75mm chamfer.
  2. Create a plane at a 1mm offset from the face the thread will begin from. Start a new sketch and use convert entities to reference the circular edge of the shaft, sketch a line across the diameter and along the front plane (set it for construction).
  3. Insert the metric die library file by drag and drop.  Set the front plane as the placement plane.  Select M10x1.0 from the list of configurations.  For the reference point, use one of the endpoints from the line in step 2. Check that the orientation of the sketch is as shown below, the sketch may be in the wrong orientation depending on the point selected for placement.
  4. Create a helix using the edge reference from the sketch in step 2.  Set the pitch to 1.0mm and length to 10 revolutions.  Adjust the start angle so the helix starts at the same location as the sketch for the thread in step 3.
  5. Use the swept cut feature selecting the .sldflp sketch as the profile and the helix as the path.
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Use this method for threads of any type that have been setup as a library feature. Saving newly created library features to the thread profiles folder location makes them accessible using method 1.

Tapered Threads

The same three methods can be used for creating tapered threads. Prepare the tapered body to apply the thread and use the “Taper Helix” option, set the taper angle as appropriate for the desired thread.