Join Leon van den Heever for an in-depth discussion in this video Top-level assembly, part of Modeling a Motorcycle Engine with SOLIDWORKS.
- To get started with our assembly let's start by creating a new assembly file using assembly template. In the property manager cancel the begin assemblies properties dialogue, and let's first save our assembly, place it in the assembly components folder, and let's name it top level assembly. Now from the command manager assembly tab select the insert components command. Select the browse button and from the assembly components folder control select the flywheel and cone rod models.
So we can insert these components simultaneously into our assembly environment. In the open documents box select only the flywheel so we place it as the first component. Make sure to select the pushpin to keep this dialogue open. Click the green okay icon so the flywheel's origin is automatically fixed to the assembly's origin. Remember it is a best practice to have your first component fixed or fully defined. Now select the cone rod part from the open documents box and click anywhere in the graphics view to place it and okay to complete the command.
Notice that the flywheel part in the feature manager is prefixed with the letter F, which indicates the component is currently fixed. Let's right-click on this component and select the float option so it is no longer fixed and that we can constrain it with mates instead. From the assembly tab select the mate command and follow my lead as we get these components constrained. Make the front plane of the flywheel coincident to the front plane of the assembly.
Make the horizontal flywheel face 15 degrees from the top plane of the assembly, and if necessary flip the dimensions so the model is represented the same as mine in the graphics view. Make the flywheel's origin coincident to the origin of the assembly. Note at this stage that even though we do not have the fixed symbol prefixing the component name that it is actually fixed since the component is currently fully defined.
This is evident by the lack of the minus symbol prefixing the part name. Now let's keep going. Make the cone rod inner cup face concentric to the flywheel shaft. Add a distance mate of three millimeters to these two faces. Now click okay to close the mate properties. Select the cone rod in the graphics view and from the configuration drop down just above the context toolbar select the cone rod cup configuration as the reference configuration and select the green tick mark to accept the selection.
Select cone rod final in the feature manager. From the insert components flyout menu select the copy with mates command. Under the mates section select repeat for both, and then okay to complete the command. Select the new instance of the cone rod and change the configuration to cone rod. We now have a complete cone rod assembly. In the graphics view rotate the cone rod cup instance so we can mate the two sections together.
Control select these two faces and let's make them coincident using the context toolbar options. In the graphics view control and select the flywheel and at the same time drag to the left or right to create another instance in the graphics view. Now let's activate the mate command and follow along as I get the second instance into position. Now we will need a concentric mate between these shafts and flip the alignment. Now make these two faces coincident and these two faces parallel to align the two components with each other.
Now change the second flywheel configuration to spline shaft and again confirm your change. Now that you've seen how we've gone about this, on your own add another cone rod instance and in the same way as before mate it to the second flywheel instance. When you're done I will 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