Tutorial: how to model '' a gear '' in '' solidworks '' and show design intent
01) File, new, part, ok
02) Tools, equations, add these parameters and equations as shown
m= 6 (module)
z=20 (teeth number)
p= m*pi (pitch)
d=m*z (primitive diameter)
da=d+2*m (head diameter)
df=d-2*m (foot diameter)
03) Sketch, select front plan and draw a circle than
replace the dimension by “=” choose “da” (Rq, this is the same procedure for the rest.)
04) Fuction, extrude, 25 for the thikness
05) A new sketch in the front face than add 3 circles and in the dimension box write “=” and chose :
The first circle: “df” the 2nd “d” the third “da”.
06) Add 2 centerlines and mirror the 3rd one
Rq: Be sure that the end of the middle centerline coincide with the “d” circle.
07) Add an arc in as shown be sure always that the entities hang in the good positions.
The center in the “df” circle and and the ends on “da” and “df”
- Mirror it twice ( reference to the two centerlines)
-Add radius for the arc r=35mm,
- and for the pitch use “=p”.
- and a relation between the arc and the point of the center line.
When the sketch is fully defined (black), extrude cut and select the two contours.
Use the circular pattern function and for the number of instance write “=” chose “z”
And this is the result:
And now our goal is here to show the result of using the design intent ^^:
(tools, equations) We change the value of “m=9” and “z=28” for example.
If you enjoy this tutorial be positive and click “it worked” and “like”