Join Leon van den Heever for an in-depth discussion in this video Configuring the splines of the flywheel, part of Modeling a Motorcycle Engine with SOLIDWORKS.
- After having worked through the SolidWorks Essentials 2014 course here at Lynda.com, or if you have been working with SolidWorks for a while, you would already have been exposed to configurations. To summarize, though, in essence configurations are used to create different versions of our model within the same file. There are different ways to create configurations and the important thing to remember is that the suppression or creation of features and the changing or creating of dimensions are the main ways in which we make our configurations unique.
Remember where you can find the Configuration Manager which lists all the configurations within our file. As mentioned before, while creating fillets we will be creating a right-hand or spline version of the model so we can use it when we assemble the bottom end. Using configurations to achieve our desired results is a simple and efficient process. Activate the Configuration Manager. Right mouse click on the part name at the top of the tree to bring up the available commands and select the Add Configuration command to add a new configuration.
Name it Spline Shaft and okay to complete. Do a slow double-click on the default configuration to rename it and call it Taper Shaft. Spline Shaft should be the active configuration and is denoted as such with the tick mark being green. If it is not, double-click on the Spline Shaft configuration to make it active. At the top of the Configuration Manager is a splitter bar. By dragging the splitter bar down to the middle, the Configuration Manager now has our features listed at the top for easy access, and our configurations below that.
If we select the Taper feature in the graphics view, the Feature Manager will automatically scroll to the selected feature which is Boss Extrude Three in our case. Right-click on it and select the Parent-Child command. Here we can see the child features related to Boss Extrude Three. Since we will be suppressing this feature, all child features will also be suppressed. Right-click on Boss Extrude Three within the Parent Child dialog and suppress it. Notice the suppressed features are grayed out in the Feature Manager tree.
Double-click Type of Shaft Configuration to see what just happened, and then activate Spline Shaft Config again. To create a spline, start a sketch on the right plane, and follow my lead to create the required profile. We'll sketch a horizontal line, then angled up to the right. Next a vertical line to the top edge, and then a horizontal to the left coincident with this vertex, and then close the profile. Let's fully define our sketch.
To the top line add a dimension of 48 millimeters. To the right-hand vertical line, add a vertical relation. Then add a dimension of 1 millimeter. To the left vertical line, add a dimension of 2 millimeters. Make the bottom line 33 millimeters. Select the Sketch Fillet command. Set the radius to 50 millimeters, and select this bottom point. Now change the fillet radius to 1 millimeter, and select this bottom right-hand point.
Close the Sketch Fillet command. From the Features tab, select the Revolved Cut command, and use the top line as the axis of revolution. Complete the command, and change to a trimetric view. Select the Spline feature in the Feature Manager. Then from the Features command bar, select the Linear Pattern drop-down menu, and select the Circular Pattern command so we can path in the Spline feature around the shaft. For the axis of revolution, use a temporary axis.
The angle is 360 degrees. The number of instances is 20. Select equal spacing and okay to complete the command. Turn off the temporary axis. On the front face of the shaft, we'll add a chamfer to break the sharp edge. Use distance-distance setting of 1 millimeter and .5 millimeters, and complete the command. Select the Fillet command with a radius of .25 millimeters. From the Fly Out Feature Manager in the top left of the graphics view, select the Spline feature and the Circular Pattern feature.
Go ahead and complete the command. That's it, save your work, and in the next video we'll start on the con rod.
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