Join Leon van den Heever for an in-depth discussion in this video Building the sprocket, part of Modeling a Motorcycle Engine with SOLIDWORKS.
- Next we will model a chain sprocket. Now I will not be going into the technicalities of sprocket sizing or correct chain selections, et cetera, since our design is only conceptual. The tooth profile I use is also not to any specification and completely sketched to what looked good to me at the time. Now go ahead and open part 0207 Sprocket from the Chapter Two lesson files. I've already added a sketch with the necessary entities. The circles represent the chain and the link rollers. And the profile between the two will be used for the sprocket tooth.
Our goal is to only have to provide the amount of teeth we want on our sprocket according to a specific chain pitch, and have the sprocket outside diameter adjust automatically. Now this will allow us to use a single model to easily create configurations for different sprocket sizes and designs. Now we can easily achieve this with equations, which we have used before. I have two variables set: one chain pitch and number of teeth. Now I have linked the chain pitch dimension to the chain pitch variable, and I have added this equation to the sprocket pitch diameter.
Now using this sketch as our driving sketch, let's go ahead and complete the model. Start a new sketch on the front line. Select the inside circle from the underlying sketch, and convert entities. Extrude this. We'll go with a depth of 10 millimeters, with a mid-plane and condition. And "OK" to complete the command. Start a new sketch on the front line. Do a "Normal to". Activate the "Convert Entities" command again.
And from the underlying sketch, select the large inside circle, the two smaller circles. Zoom into the tooth profile. And then select these three lines. And then make sure these bottom two are also selected. And "OK" to complete the command. Now follow my lead and let's trim out the following. And be sure to get these two lines, as well.
You should now only have the tooth profile. Now with that, let's do an extrude. And this time we will do two directions, with "Up to surface" and conditions, so the profile adjusts with the thickness of the previous extruded feature. And also ensure that "Merge Results" is selected. Now let's do a circular pattern. We'll use a temporary axis as the pattern axis.
The angle will be 360 degrees. We'll activate the "Features to Pattern" selection box, and select "Boss Extrude" too, from the flyout feature manager at the top left of the graphics view. We want "Equal spacing" activated, and then for the "Number of instances", let's do an equals so that we can select the "Number of teeth" variable. And we will thus get the value associated with that variable as well. Now everything should update nicely in the model.
And go ahead and turn off temporary axis. Start a new sketch on the right plane. Do a "Normal to". Sketch a center point direct angle just above the underlying model. Now we will use this to cut the chamfers on the teeth to allow easy meshing with the chain. Add a dimension to the vertical left edge of 15 millimeters. Make the left edge one millimeter from the top, left vertex.
Rotate the model slightly, so we can see the driving sketch beneath it. Now select the center line of the rectangle, and then the top horizontal line of the tooth profile, so that we can pierce the relation. If needed, add a vertical relation between the center of the rectangle and the origin. Select the bottom, horizontal line of the rectangle. and let's change this to construction since we don't need it. Add a horizontal, center line from the origin out to the left, and we'll be using this center line for our axis orientation.
And make this left vertex vertical to the bottom, left vertex of the erect angle. And now with the origin line selected, go to "Features", select "Revolve Cut", and then for the contours, select each triangle. And "OK" to complete the command. Now if needed hide any sketches to tidy things up. On the front plane, start a new sketch, and place a circle with a diameter of 50 millimeters onto the origin.
Extrude this 14 millimeters, use a mid-plane, and "OK" to complete the command. Again add another sketch on the front plane. And place a circle with a diameter of 23 millimeters on the origin. And now do a "Cut through all, both". And complete the command.
Now from this design, we should be able to create a nice variety of sprocket sizes and styles needed. Now review the equations used in this design to ensure you understand what they are doing, and I'll see you in the next video.
Need a better background in SOLIDWORKS before you can continue? Check out SOLIDWORKS 2014 Essential Training.
- Sketching the flywheel
- Building and cutting the flywheel shafts
- Filleting the flywheels
- Splitting the connecting rod
- Building the sprocket
- Modeling the camshaft
- Combining parts into an assembly