Join Leon van den Heever for an in-depth discussion in this video Building the shafts of the flywheel, part of Modeling a Motorcycle Engine with SOLIDWORKS.
- We will now use the "Revolve Boss Base" command to revolve the front shaft of our flywheel. The reason for using this tool instead of the "Extrude Boss Base" is so we can capture our required profile from a single sketch and extrude. Start a new sketch on the right plane. Using the "Spacebar" key to bring up the in-context "Do Your Orientations" dialog, we have easy access to the "Normal to" icon, which rotates the graphics view normal to our screen. Note the shortcut key is "Control+8", if you prefer to use that instead.
Select the icon for a normal-to orientation. Follow my lead as I sketch the required profile, select the line tool, starting on the midpoint of the front edge of the underlying geometry. Sketch a vertical line, then a horizontal. Add a couple of steps similar to this. Add another horizontal line, then a vertical line down 'til we are perpendicular with the origin, which is denoted for us by the blue inference line and then back to our start point.
Note that the reason I started on the front edge of the existing extrude, and not on the origin, is so the front shaft will maintain its length, relevant to that first. If the underlying extrusion depth had to change, if we used the origin instead, it would simply be fixed by that and give us undesired results. "Escape" to cancel the active command. Make the first step's vertical and horizontal lines equal to each other, so we only need to apply one dimension.
Select the "Smart Dimension" tool, set the right vertical line to 43 millimeters, the top horizontal line to 64 millimeters, step one to six millimeters, step two to 12 millimeters, and this horizontal line to 54 millimeters. From the "Features" tab, select the "Revolve Boss Base" command. Note the "Axis of Revolution" box is preselected in the command's properties, since we need to specify an axis.
Whenever I am adjusting feature properties, I prefer to change my graphics view to the default tri-metric view, so I can properly see the result of my extrusion for additional adjustments, if needed. We will select the bottom horizontal line in the graphics view as our axis of revolution. Complete the command. On the front face of the newly-created extrusion, we will create another extrusion. With the face selected in the graphics view, from the context toolbar, select the "Sketch" icon. With the face still selected, select the "Convert Entities" command, which automatically creates a circle from the underlying geometry.
Now if the underlying geometry changes, so will the sketch. Do an extrude. Make the length 32 millimeters, with a draft of eight degrees, and complete the command. Note I activated the draft dialog by selecting this "Draft" icon. Let's do the back shaft while we are at it. On the back face of our flywheel, start a new sketch. And sketch a circle with its center point vertical to the origin. Create a vertical relation from the center point to the origin, so the circle is constrained in that position.
Make the circle equal to the top arc. Dimension the circle 60 millimeters from the origin. Extrude the circle 50 millimeters, and your model should now look like this. We'll leave it at that 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