Join Leon van den Heever for an in-depth discussion in this video Building the details of the connecting rod, part of Modeling a Motorcycle Engine with SOLIDWORKS.
- Let's continue with our cone rod design. And I changed the view orientation to a bottom view. And start a new sketch on the right, flat, bottom face. Select the center point slot command. And from the origin sketch I slot something like this. We will use the flip side of the slot, to cut around into the sides of our model. Now zoom in to this area to make it easier to select. And make this vertex and the slot arc coincident to each other.
Next control, select the top line of the slot, and the underlying circle edge, and make them co-linear to each other. And from this we can do an extruded cut command. Let's use a through-all and condition. And make sure to select the "Flip side to cut" option. And go ahead and complete the command. Let's start another sketch on the same face. This time sketch a circle.
And do this on both flat faces. Let's make them equal to each other. And also add a horizontal relation between the circle centers. And also a horizontal relation between one of the centers and the origin. Sketch a center line vertically from the origin. "Control+Select" the right circle center, the center line, and the left circle center, and let's add a symmetrical relation.
"Dimension" one of the circles to 12 millimeters. And then "Shift+Dimension" the circle edge to the underlying arc to six millimeters. Do an extruded cut, and condition will be "Through all", and "OK" to complete the command. Go to "Features", "Reference Geometry", and let's add a plane for our next sketch.
Use the top plane and parallel for the first reference, and the inside face of the bottom circle as the second reference. And this should be tangent. Flip the plane if you need to, so it is above the default top plane. Okay, and start a new sketch on this plane. And we will use this to create a countable to our existing holes. "Control+Select" these two top edges of the right hole, and do an outside, offset entities of three millimeters.
Let's do the same for the left hole. Do a blind extruded cut. Let's make this 40 millimeters in an upward direction. And "OK" to complete the command. Now let's tidy up a few things. Add a 25 millimeter fillet to the recess profile, to this bottom edge, and don't forget to do the back recess, as well.
While our setting is at 25 millimeters, let's also do these edges on the top arc. Add a 100 millimeter fillet to the left and the right edges of the recess cut. And again, the back recess as well. Let's add a 10 millimeter fillet to these bottom edges, and we'll leave it at that.
Save your work 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