Cosmetic threads are a quick and lightweight method of indicating threaded components in a design. The screw mate option cannot be used as these threads to not contain any geometry.
Internal Threads – Hole Wizard
- Use a sketch containing fully defined point location(s) where the holes are to be placed, then exit the sketch. Refer to the comment in step 7.
- Click on the “Hole Wizard” button from the features tab.
- Select the option for a straight tap from the hole type selection. Set the standard and type options appropriate to the thread being used. Use ANSI metric and bottoming tapped hole for this example.
- Choose the appropriate size of hole from the hole specifications section. M10x1.0 will be used.
- Set the desired end condition for the hole. Select blind for holes that do not pass through the entire body, otherwise use through all.
- In the options section select the cosmetic thread option and tick the box to include a thread callout.
- Switch to the positions tab to specify the location of the hole. Select the face to place the hole on, then click anywhere on the surface a hole is required. Holes can be placed without a pre-existing sketch, however their positions will not be fully defined, edit the sketch to fully define the hole positions. Tip: to place a hole that is concentric to a curved body hover over the circular edge to display the center of the curve, place the hole on that point and it will be constrained.
If the cosmetic thread does not appear select “Tools” – “Options” and select the detailing section of the “document properties” tab. In the display filter ensure cosmetic threads and shaded cosmetic threads are selected.
External Threads – Insert Callout
To create a cosmetic thread on a shaft another option is required use “Insert” – “Annotations” – “Cosmetic Thread…” . Use the following settings:
- Circular Edges – Select the desired edge in the thread settings.
- Select the face the thread starts from (Only applies to the blind end condition).
- Standard – Choose ANSI metric.
- Type – Machine threads.
- Size – M10x1.0.
- End condition – Blind.
- Length – Set the desired length of thread to be applied (Only applies to the blind end condition). Use 20mm for the example.
Custom Thread with callout
Select “none” from the standard list if the desired callout is not available in SolidWorks. Input the thread designation in the thread callout box.
Create a hole to the desired diameter. Instead of inputting a minor diameter use the value of the major diameter.