Join Leon van den Heever for an in-depth discussion in this video Cutting the back of the flywheel, part of Modeling a Motorcycle Engine with SOLIDWORKS.
- We will continue with a couple more cuts to the back of our flywheel. We will do another revolve feature, only this time we will use the revolved cut command. Let's start a new sketch on the right plane. Rotate the view normal to. Follow along with me and sketch the following profile from the bottom vertex of the underlying geometry. Draw a vertical line up, a horizontal line to the left, an angled line slightly down like this, a vertical line down and coincident with this bottom edge, and close the profile back to the vertex.
We will use this profile in the revolved cut command, but let's first fully define the sketch since fully defining our sketch is a best practice and we will use dimensions to do this. Make the top horizontal line 12 millimeters, the left vertical line 21 millimeters, the right vertical line 26 millimeters, and add an angled dimension to the inside of these two lines of 107 degrees.
Our profile is now fully defined, and we can tell this by the fact that all the lines are black in color. Next, a horizontal center line is needed which will be used as an access of revolution in the revolved cut command. With the view still normal to the right view, select the bottom edge of the back shaft so we can convert it into our existing sketch and saving us from having to sketch new geometry with the line tool. To do this with the bottom edge of the back shaft selected, select the convert entities command, and then change the solid line to a center line by selecting the converted line.
From the context toolbar, select the construction and geometry toggle icon. Next, select the revolved cut command. Set the end condition to be midplane so the cut will be symmetrical. And set the angle to 140 degrees. Go ahead and complete the command. Before making our second cut, we need to make the first sketch of our part visible so we can reference it in our next sketch. In the feature manager, expand the boss extrude one feature.
Click on the sketch icon, and select the glasses icon from the context toolbar which shows or hides the sketch. Note, we can now see the sketch in the graphics view, change the orientation to a back view, and start another sketch on this back face. Select the three point arc command, and use the endpoints of the underlying horizontal line to constrain the arc ends. Get the arc to look something like this, and click to complete the arc.
Escape to exit the command. Now control select the arc, and the edge and add a concentric relation between the back shaft outer edge and the arc. We will use the convert entities again to create sketch entities from the underlying geometry. Activate the convert entities command. Select the center circle, the left edge, the right edge, and right-click to complete the command. Let's sketch a horizontal line between these two points to split the circle down the middle.
Now we will use the trim entities command to trim off what we don't need. With the command selected, simply drag across the geometry you no longer need, follow my lead, and you should end up with a closed profile like this. Select the extruded cut command. Set the end condition to up to vertex to allow us to use a vertex to extrude up to.
Rotate the graphics view like this, and select the vertex over here. Using this point, the cut depth will always be relevant to the underlying vertex position which is exactly what we want in this instance. Complete the command, save your work, 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