Join Leon van den Heever for an in-depth discussion in this video Cutting the shafts of the flywheel, part of Modeling a Motorcycle Engine with SOLIDWORKS.
- In this video, we will do a number of cut extrudes to our model. Let's start by changing the view orientation to a back view. On the face of the back shaft, let's create a new sketch for our first cut. With the first stall selected, select the keyboard shortcut "S" to bring up our context toolbar and select the "Offset Entities" command. In the property manager, enter an offset of nine millimeters.
And just below that, select the "Reverse" direction option, so the sketch is created to the inside of the selected face. Go ahead and complete the offset command. If we are going to use a specific view frequently during our design, we can create our own saved views for repetitive use. For now we will set up two such views. Select the "Spacebar" to bring up the orientation window. Let's keep this dialogue visible for now by selecting the "Keep Visible" icon, since we want to add multiple views.
Change the graphic view to be similar to mine. In the orientation window, the second icon at the top left is the "New View" icon. Select it and name the view "Back angled" and select "OK". Again, rotate the view similar to mine, and name this view "Front angled" and select "OK".
You will now have both these newly-created views in the orientation window for easy access. Select the "Keep visible" icon to turn it off. Select the "Spacebar" and select the back-angled view. This is so we can see the result of our cut for necessary adjustments. To cut the hole select the "Extruded Cut" command, and set the depth to 25 millimeters, and complete the command.
Again, change the orientation to a back view. Select the inside bottom face of our first cut, and start a new sketch. Again use the "Offset Entities" command, using an offset of 10 millimeters, and reverse the direction and complete the command. Select the "Spacebar" and select the front-angled view to view our model from our saved orientation. Select the "Extruded Cut" command and this time, we will use an "Up to surface" and condition, up to this face.
We do this so the cut will always go through all geometry up to this face, irrespective of how our model changes down the track. If I did not move my mouse when selecting the face, note the feedback on my mouse cursor. It is telling me that if I do a right mouse click, I can complete the command. This is another efficiency tool for us. I'm going to go ahead and do that. And we'll use this often during our modeling. So if you wonder how I completed a command so quickly at times, it's probably because I use this to my advantage.
Again, change the orientation to a back view. Start a new sketch on this face. Select the inner cuts edge and offset entities again with an offset of five millimeters. And no need to reverse direction this time. Complete the command. "Spacebar" and select the front-angled view we created, since we will need to select the same face as in the previous cut feature.
Select the "Extrude Cut" command. The and condition should again be an "Up to surface" and condition. And we will select the same face as before. Again using this and condition for the same reasons as before, as well, go ahead and complete the command. Next we will turn our attention to the front shaft. Select the front face of the front shaft, and start a new sketch. Select the "Offset Entities" command.
Use an offset of seven millimeters and reverse the direction. Complete the offset command. Select the "Extruded Cut" command, and set a blind depth of 30 millimeters. Complete the command. We will wrap it up with that, and I'll see you in the next video where we'll complete the remaining cuts.
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