Join Leon van den Heever for an in-depth discussion in this video Shaping the arc, part of Modeling a Motorcycle Engine with SOLIDWORKS.
- Next, we want to add some shape to the top arc of our flywheel. We're going to sketch our next profile on the right plane, and the reason I've chosen this plane is that I intend using the Revolved Cut command, and I know that it has a Mid-Plane End Condition which we can use to cut our arc profile symmetrically. We need to plan ahead a bit in that we want the bottom of our next profile to be collinear with the very top of the circle extrude. However, we have already removed material from the top of the circle extrude with the holes we cut through the top arc.
This is one of the powerful aspects of parametric modelers that we can roll back to a point in time to add, remove, or change geometry. Within the Feature Manager, we can select a feature and from the Context toolbar, roll back to and including the feature we selected which in our case will be the first cut feature we made. Now we can access the top of the circle geometry, and can get started on our Revolved Cut profile. Let's start a new sketch on the right plane.
Let's get our view Normal To, and zoom in to the top arc section where we'll be sketching our profile. With the Line command selected, start from this vertex which is the very top of our circle's extrude, and drag a line vertically up terminating it near this top edge. Exact alignment is not necessary since we will add a horizontal relationship between these two vertices like this. Now from the start point, sketch a short horizontal line, and let's dimension it to 4 millimeters to fully constrain it.
Next select the Style Spline command from the Spline Fly Out menu. Start the spline by placing the first point on the right end of the horizontal line. Place the next point to the right and slightly up. Place the third point something like this, another about here, and the last point coincident to the top edge like this. We will sketch a horizontal line between these two points to close the current open profile. What we're aiming for is a nice even-curved profile spline, and the Style Spline command makes it a simple process.
Let's proceed to fully define our profile. Add a 20 degree angle between the bottom horizontal line, and the bottom spline line. Add a vertical relation to the vertical line. Add a mid-point relation to this point and this edge. Add a 7.2 millimeter dimension from the top point to the back edge. Add a 4 millimeter horizontal dimension between the center and top mid-points.
And finally, add a 14.4 millimeter vertical dimension between the top and mid-points as well. Our profile is looking good. Let's select the Revolved Cut command. Rotate the view to Default Trimetric and zoom in a bit. As we already know, we need an axis of revolution, but we have not sketched one as we did in previous sessions. Well, this time to save us time, or unnecessary sketched geometry, we will go to the Heads Up View toolbar, and from the Fly Out toolbar of the Hide-Show icons, select the View Temporary Axis icon to show the axis.
What you'll notice in the graphics view, is that all cylindrical features always have a temporary axis that we can toggle the visibility in this manner. Note the blue axes on all cylindrical features. The great thing about this is that we can actually use these temporary axes to constrain to. This can be a huge time saver. Let's select the circle's axis as the axis of revolution for our Revolved Cut. Make the End Condition mid-plane. Hence the reason we started our sketch on the right plane, and for a symmetrical cut to our model.
Use a 180 degrees for our angle. Go ahead and hide the temporary axis. Select the visible sketch in the graphics view, and from the Context toolbar, select the glasses icon to hide the sketch. In the Feature Manager, right mouse click anywhere in the grayed-out region below the blue rollback bar, and select Roll to End from the menu to again show all our features. You can go ahead and save your model, and in the next video we'll add some fillets to tidy up our design.
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