Join Leon van den Heever for an in-depth discussion in this video Modeling the camshaft, part of Modeling a Motorcycle Engine with SOLIDWORKS.
- For our last part, we will complete the camshaft. And to get started go ahead and open the file Camshaft_Start from the Lessons folder. We have a few simple extrusions and a hole pattern. And we are gonna go ahead and mirror the existing body about the back face of the shaft. So we can have two cams. And we gonna make sure that Solids or Merged Solids rather is selected. Now on the back face, we will do a circular extrude.
And we are gonna use Convert Entities to pick up the underlined shaft edge. And let's do a blind extrusion and let's set this to 40 millimeters. Now to the end of this shaft, we're going to go ahead and add a triangular mounting flange. So we will start a new sketch on the back face of the shaft. And I'm gonna go ahead and select the existing sketch called SketchTriangle from the Feature Manager. And let's do a Convert Entities. With this done, let's do an extrusion.
And we will go for a blind end condition of 10 millimeters. On the front face of the triangle, let's start a new sketch. And again we gonna offset entities of the back shaft edge and we'll go for four millimeters. With this we'll do a Boss-Extrude and let's go for two millimeters with a blind end condition. And on the back face of the triangle, let's do a circular extrude. Again we'll use Convert Entitles from the shaft.
And with that implies we'll do a blind extrusion at 20 millimeters. Now let's do an extruded cut through the entire shaft. And we'll use a diameter of 15 millimeters for this. We will need some threaded bolt holes. For this we'll select the back face of the triangle. And on this occasion, we gonna use the Hole Wizard.
You can find this on the Features tab. And I'm gonna create a straight tapped hole. We will use an Antimetric standard. And for type let's select Tapped Hole. For size let's use and M8x1.0. And also make the thread Up To Next. Under options, we will use Tap Drill Diameter. And at the top, let's select the Position tab. Select the Line command and sketch a center line from the origin to the center of the left arc of the triangle.
Select the Point command and add the point coincident to the center line. And then I'm gonna go ahead and dimension this seven millimeters from the arc. When done, complete the command. And we'll now do a circular pattern of this hole. And let's make sure again Equal Spacing is selected. And we will use three instances.
Okay, do you complete the command? And that's pretty much our shaft done. Again add your fillets and chamfers and I'll see you in the next chapter where we will start on our assembly.
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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