Nick, Here are three ways.
Method 1 - In the drawing as a cosmetic thread. Easiest way is an Annotation in the Drawing.
Select the major diameter circular profile in the drawing.
Select Insert, Annotations, Cosmetic Thread or select Cosmetric Thread from the Annotations toolbar. If you have the CommandManager displayed you have to toggle between Annotations, Drawings and Sketch toolbars in the Control Area (leftside) of the CommandManager.
To display toolbars, right-click in the gray area next to Help in the Main menu and check the Annoations toolbar.
Enter the minor diameter, Select Blind (probably), Thru All (for holes) or Uptonext (requires a face)
Method 2 from the Hole wizard - cosmetic thread option only works if you have a hole. Not your current example - but this is handy when you have interior holes. Lot less time and looks good for a picture file.
Method 3 - If you really need the thread feature, example a plastic bottle, you have to create a Sweep feature.
The Sweeep feature uses 2 sketches, path and profile. The path is a helical curve and the profile would be the thread cross section. This takes the most time and it should only be used when you really nead the thread as a feature and not an annotation.
Here is a simple example:
Create a cylinder on the front plane as an extruded base feature.
For the path,
Select the front face of the cylinder and select sketch to open a new sketch.
Click Convert Entities from the Sketch tools toolbar.
Select Insert Curve/Helix from the Main menu.
Enter pitch and number of threads.
Key point - Select the start angle at 90 (for cross section sketch on the right plane). Click OK to exit the Helix.
Save and exit sketch1, green check mark.
For the second sketch, profile,
Click the right plane and open a new sketch
The simpliest thread profile to illustrate a sweep is circular, but usually they have a tooth shape.
Display an Isometric view so you can see your helix and the sketch on the right plane.
Sketch a circle on the right plane, above the helix.
A Sweep requires a Pierce relationship.
Select Add relations from the Sketch toolbar. Select the center point of the circle and select the helical curve. Select Pierce.
Save and exit the sketch, this is sketch2.
You now have 2 sketches in the FeatureManager. The small circle is attached to the helix.
Select Sweep from the Features toolbar, select Sketch1 for the profile, select Sketch2 for the path.
You should also create a threadplane offset from the start of the thread so you can adjust the starting depth - but that is another lesson.
Regards, Marie