Join Leon van den Heever for an in-depth discussion in this video Detailing the piston, part of Modeling a Motorcycle Engine with SOLIDWORKS.
- Continuing on with our piston model, let's go ahead and add a reference plane to the bottom shelled face of the model. Let's set this to a distance of two millimeters upward and ok to complete the command. You can resize the reference plane if you like, and we'll use this for a numbers of ribs and the bearings support as well. Now start a new sketch on the reference plane. We'll do a normal to, and let's sketch a center line vertically.
Sketch a centerpoint rectangle, and then we'll sketch two vertical lines in the rectangle. One on the left, and the other on the right. Add a dimension of 49 millimeters to the right vertical line. Make the distance between the two right vertical lines 22.5 millimeters, and from the origin to the first right vertical line we'll make this 17 millimeters.
Make these three lines symmetrical, and then let's trim out these three horizontal lines. Do an extruded boss to the top, inside face of the model, and ok to complete the command. Now start another sketch on the reference plane. We'll sketch a center line vertically, and another one horizontally.
Now sketch a solid line something like this. We'll dimension the bottom vertex of this line to the right vertical edge of the underlying geometry to five millimeters. Add a vertical relation to the top vertex and left top vertex of the underlying geometry. Next, mirror this line across to the right and then the two top lines to the bottom.
From the features tab, activate the rib command. Set the rib thickness to five millimeters, and ok to complete the command. Make the sketch of rib one visible so we can reference it in the next rib sketch. On plane one, start a new sketch. Sketch a horizontal line between the top, two angled lines from the underlying sketch and order relate the horizontal line to the centers, something like this.
Now do the same for the bottom. Let's do another rib command, again five millimeters, and ok. Now we can hide the sketch of rib one, and we can also hide plane one to keep our graphics view tidy. Change to a bottom orientation view. Now for the last rib, start a new sketch on this bottom, recessed face.
The following will be similar to the first rib sketch we created. A horizontal center line should do for the mirror. Sketch the first line like this. Add a dimension of five millimeters to this vertex and this edge. Make the two top vertices horizontal, and sketch a similar line on the right side.
Make the two bottom and top vertices of each line horizontal to each other. Mirror these two down to the bottom side, and now add a five millimeter rib again. To cut a profile through our ribs, start a new sketch on the right plane. Normal to and sketch a vertical center line from the origin down.
Sketch a center rectangle on the bottom point of the vertical line. Dimension it 85 millimeters horizontally, and 10 millimeters vertically. Do an extruded cut, through all both and ok. Now for the bearing holes, let's do a new sketch on the right plane. We'll go normal to. Change the display style to hidden lines visible.
Now sketch a circle vertically below the origin. Add a vertical relation, and dimension the circle to 27.8 millimeters. Next do a shift dimension from the circle's edge to the top inside edge, and let's set this to 10 millimeters. Change your display to solid with edges again. Now do an extruded cut.
We'll go up to surface in two directions, and then select the outside rectangular faces. On the top of the piston, sketch a center rectangle on the origin, and set a vertical dimension of eight millimeters. We will use one of the edges as a plane reference. Complete the sketch. Make the sketch visible, since we need to reference it.
Now create a new reference plane using the bottom rectangle line as the first reference. As a second reference, use the top plane and set it to an angle of three degrees, and ok to complete the command. On this reference plane, start a new sketch, which will be the valve location on the piston. Do a normal to, and let's sketch a vertical center line down from the origin.
Sketch a circle on either side of the vertical line. Let's make them equal. Make them tangent to the underlying rectangle sketch. Now sketch a horizontal line tangent between the top of the circles. Make the circles tangent to the vertical line, and then trim out these two segments.
Do an extruded cut, through all, and in an upward direction, and ok to complete the command. Add a one millimeter fillet to the five corners and the two outside edges of this cut. Now let's mirror the cut and the fillet feature across the right plane, and that should complete our piston.
Again, I'll let you take the time to add the necessary chamfers and fillets to the model, 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