Join Leon van den Heever for an in-depth discussion in this video Roughing out the piston, part of Modeling a Motorcycle Engine with SOLIDWORKS.
- To start on the piston model, from the Chapter Two folder open the 02<u>04</u>Piston<u>Start</u>Part file. We have a simple circular extrude as our starting point. On the right plane, start a new sketch. Now go Normal To. We will cut the grooves for the piston rings. Use a center rectangle and start coincident to the left edge. Make the horizontal edge 2 millimeters long. Position the center of the rectangle 10 millimeters from the top edge of the underlying geometry.
Let's make the groove width 3 millimeters. Now do a revolved cut, and using a temporary axis we'll cut a groove around the model. From the Feature tab, select the Linear Pattern command. We need three of these grooves, and instead of sketching and cutting them, and for additional flexibility, patterning is a better option. Select the Assign Temporary Axis again, and this time as our pattern direction.
Reverse the direction so the direction arrow is pointing down. Set the spacing to 5 millimeters and the instances to 3. Select the Features To pattern box, and in the graphics view select the bottom face of the groove we just cut, and okay to complete the command. Go ahead and toggle off the temporary axis. Let's turn this into a thin-walled model using the Shell command found on the Features tab.
We'll use a thickness of 10 millimeters. Select the Faces to Remove box and in the graphics view select the bottom face of our model and okay to complete the command. On the bottom face of our model start a new sketch. Select the inside circular edge, and do an Offset Entities outward at 5 millimeters. Next do an extruded cut. We will do an Up To Surface, and if you zoom to the inside of the model you will see a small ridge.
Use this surface as the Up To selection. Again, on the bottom face, we'll start another sketch. Run the Convert Entities command, and select the outer two edges. Sketch a centerline vertically and horizontally. If you select Boss Extrude One from the Feature Manager, you can hide the underlying geometry to make things easier to see. Connect the two circular edges with two additional line segments like this.
I'll use these vertices to create symmetry. Add a dimension to the two short lines of 107 degrees, and then let's turn off the bottom sections. Right-click on one of the solid entities and select Chain, and then mirror the profile down to the bottom. Do this about the horizontal line. Exit the sketch and show Extrude One again.
With the sketch we just created selected, do an extruded cut. Use an offset from Surface End Condition. Select this bottom face and make the offset distance 2 millimeters. And select the Flip side to cut option, and okay to complete the command. Now on the front plane, start a new sketch again. We'll go Normal To. We want to add a bit of profile to the remaining sides.
Let's add a three-point arc between these two edges. Add a 55 millimeter radius to this. Make the top point to edge a distance of 12 millimeters. And the bottom vertices 12 millimeters as well. With the line tool, close the profile, and let's add a vertical centerline so we can mirror about it.
Now let's do a Chain Select again on the Entities, and then we'll mirror the profile across the vertical line. Now let's do an extruded cut through all both, and okay to complete the command. We'll continue the rest in the next video.
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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