Join Leon van den Heever for an in-depth discussion in this video Filleting the flywheel, part of Modeling a Motorcycle Engine with SOLIDWORKS.
- For the finishing touches to our model, we will now add a number of fillets. Since fillets create faces and edges that can be used to create additional fillets, the order in which we create them is important, and sometimes if a fillet does not solve as expected, repositioning it in the feature manager may help. It is not a necessity, but for similar reasons, and if you intend using different size fillets, try to create your larger fillets, first. And finally, leave cosmetic fillets until the end of your model's design, so they can be easily suppressed, without affecting other features, if needed.
With this in mind, let's get to it. From the features command bar, select the "Fillet" command. With a "Radius" entry box preselected, enter a value of 20 millimeters, and "Enter" once. Make sure you have the fillet type set to "Constant size". It is, of course, always useful to have full preview active when possible, so we can get feedback from the graphics view on our adjustments and selections. Select these two edges and complete the command. Next we will add a 30 millimeter radius to these two edges.
Add another fillet feature. Let's set the size to eight millimeters, and apply it to these three edges. Next we want to add a four-millimeter fillet to this edge, but we need to create a bit more room for it. Select the surface to display the feature's dimensions, click once on the radius dimension, and change it to 40 millimeters. Now add another fillet. Set the size to four millimeters, and select this inside edge.
"OK" to complete the command. The next fillet feature will be one millimeter. Select these three edges and these two faces. "OK" to complete the command. At the tip of the front shaft, we want to add another one-millimeter fillet. And we could've added it to the one-millimeter fillet feature we just created. But thinking ahead, we will use this same model to create a right-hand version with splines instead of the taper feature at the shaft's end.
And since we will use feature suppression, it will be cleaner to keep these fillets separate. Add another fillet to this face with the radius of one millimeter, and "OK". If we take a look at the first one-millimeter, fillet feature properties, we can see that the tangent propagation option is activated for the selected edges. Let's cancel out of this feature. We want to add another one-millimeter fillet to this edge, however this time turn off tangent propagation since we only want the single edge affected.
"OK" to complete. "Spacebar" and change to a back-angled orientation, so we can add a final fillet feature to the back of the model. Select this face, then the fillet feature command from the context toolbar. Make sure the radius is one millimeter, and add these five faces. And lastly, select the inside edge of the back shaft. "OK" to complete.
That completes our model design. 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