Join Leon van den Heever for an in-depth discussion in this video Creating additional gears, part of Modeling a Motorcycle Engine with SOLIDWORKS.
Next, we are going to use the previous sprocket and a configuration to create the large sprocket for our chain assembly. Now, we'll be getting to assemblies in chapter three of our project. For now, do a Save As Copy and open and name the file Sprocket Final Configs. And go ahead and save that. Let's start by adding a new configuration.
Select the Configuration Manager. We will right-click on the part name and select the Add Configuration command. Let's name it Large Sprocket and then we'll say OK to that. This configuration is now automatically activated for us and to easily access the features, we will split our Feature Manager. Now, click on the Cut Extrude1 feature, so we can see the dimensions in the Graphics view and let's change the dimension to thirteen millimeters.
Sketch a circle on the front face of Boss Extrude3, which we will use for a boss extrusion. And let's offset it five millimeters from Cut Extrude1's edge. Also, let's then do a Convert Entities on the same inch and let's go ahead and extrude this twenty-four millimeters. We'll go with a Blind End Condition and make sure that we're extruding to the front.
Let's edit Boss Extrude3 so we can make some changes that are only relevant to this configuration. Change the End Condition to Blind and set the distance to seven millimeters. Now, go ahead and activate Direction2 and do a Blind Extrude to twenty millimeters. To the bottom of the Properties Manager, we have Configuration Options.
Select the This Configuration option and now we can go ahead and complete the command. Sketch a circle on the front face of Boss Extrude1 and roughly vertical to the origin. We will cut away some of the material to make the sprocket lighter. Let's constrain the center of the circle vertically to the origin and let's also add a twenty-five millimeter diameter.
Add a forty-five millimeter dimension between the origin and the center of the circle and let's go ahead and do an extruded cut and we will use a Through All End Condition. Let's pattern this hole. Under the Linear Pattern flyout, select the Circular Pattern command. Use a temporary axis for the pattern axis.
Let's select equal spacing and set the number of instances to six. Okay, you complete the command and let's go ahead and turn off the Temporary Axis again. That's it. Go ahead and add fillets and chamfers as before and when you are done, save your work. In this same manner, I will create additional gears and sprockets, which we will use during the assembly of our design. I'll see you in the next video where we'll be modeling the final part before assembling our project.
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- 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