Following the previous tutorial on creating external (Male) threads in SolidWorks, this tutorial will outline the procedure for creating internal (female) threads. Wherever possible use cosmetic threads over modeling each thread. Cosmetic threads require less computer resources and can be applied easily. Only model threads if they are critical to the design.
There are various methods that can be used to create female threads. The insert thread feature, for example, is the easiest.
Insert Thread Feature
The following example will use an M10x1.0 thread. Create a hole feature and set the dimension value to that of the minor diameter. The step to include a 0.75mm chamfer, on both ends of the hole, is optional. Use “Insert” – “Features” – “Thread…” or expand the drop down from hole wizard and select “Thread”. Follow the instructions below to create the threaded cut:
- Edge – Select the edge of the hole from which the thread will start.
- Offset mm – enter a value of 1mm and use flip direction so the thread starts from above the hole. Adjust the offset value to suit the thread pitch that is required. This will create a smooth transition out of the hole at both ends, otherwise the thread will end abruptly.
- Offset angular – This option changes the starting location of the thread. Set it to 0° for this example.
- End condition/length – Set the end condition to blind and the length to 15mm. Other combinations are revolutions/up to selection, they are used to specify the length as a number of revolutions or up to a selected face respectively.
- Type – Select Metric Tap as they are for female threads. Alternatively, select tap option for another thread standard.
- Size – set the size to M10x1.0 or to the required thread size.
- Thread method – select the cut option.
Begin by creating a sketch of the custom thread profile. This method is useful when using a non standard thread profile or one that is not available through the SolidWorks library files. This method involves the use sketch of the thread profile and creating a swept cut. Instructions for creating this type of thread are outlined below:
- Chamfer ends to 0.75mm (optional).
- Offset a plane 1mm above the face where the thread will start. This will create a smooth transition into and out of the hole.
- To create a helix, a sketch is required. This sketch needs to be a circle located on the plane from step 2. Convert entities can be used to project the edge of the circle onto the plane.
- From the CommandManager select “Helix and Spiral” from the “Curves” drop down menu. Adjust the helix for a pitch of 1.0mm and 20 revolutions, or to suit the thread to be inserted. Leave the thread direction as clockwise.
- Create the desired thread profile, if a standard is available consult the thread charts for that standard. Constrain a point in the sketch to the helix using a pierce.
- Select the swept cut feature from the CommandManager. Use the sketched thread profile and the helix as the profile and path respectively.
This method can be used for threads of any type.
Tap Library File
Instead sketching a thread profile, make use of the available SolidWorks library files. The files can be found in “C:\ProgramData\SOLIDWORKS\SOLIDWORKS 20XX\Thread Profiles”. There are two methods to insert these sketches, both involve dragging and dropping the files. If the folder path listed above is set as part of the design library, use the Task Pane and browse for the thread profile. Alternatively open the path in file explorer and drag and drop the .sldlfp file into the part being edited. Follow the steps below to create a thread using this method:
- Optional 0.75mm chamfer.
- Similar to the previous two methods, create a plane 1mm above the face that the thread will begin from. As this method also requires a helix, a sketch with a circle will be required to define the helix. In a new sketch, use convert entities to project the circular edge of the hole onto the plane that was just created. In the same sketch include a construction line across the diameter and along the front plane. This line will be used to locate the sketch of the thread profile.
- Drag and drop the metric tap library file into SolidWorks and select the front plane for placement. Select the desired thread size from the list of configurations, use M10x1.0 for this example. Select one of the endpoints from the line in step 2 as the reference point. As there is no option to locate the profile, verify the sketch orientation is correct before clicking the green checkmark.
- Use the circular reference from step 2 to create a helix. Use 1.0mm and 17 revolutions for pitch and length respectively. Ensure the starting position of the helix and the placement of the sketch in step 3 are at the same location.
- Create a swept cut feature, use the sketch from step 3 and helix from step 4 as the profile and path.
This method also requires a library feature, therefore the insert thread method is preferred. These library features can be stored in the same directory and become available from the insert thread options.
Tapered threads only differ in the shape of the hole, the same three methods can be used to create tapered threads. Create a tapered hole to apply the thread. In the options when creating the helix, select the “Taper Helix” and input the required angle for the desired thread.