We will build this part within the assembly environment, rather than switching to the part environment. The top base is to be created within assembly because we need to use other components as reference geometry.
In this exercise we will work with both solids and faces.
Steps to Follow:
1. Add empty component
2. Create sketches
3. Create faces
4. Trim faces
5. Round edges
6. Create cylinders
7. Mirror
8. Create shell
9. Create center hole
Step 1 - Add New Component
Click the 
icon, or open the popup menu and select Add New. Select the Part option.
The Profile Card dialog appears; assign the name top base. Place this new part By Pick anywhere in the assembly. The UCS of this new part appears.
The top base component must be activated in order to work on it.
Right-click on top base in the tree, and select Activate Component from the popup menu. (Or click the 
icon or select Environment / Activate / Component.)
All other components are now displayed in "de-activated" mode.
To organize a comfortable working environment, hide all objects except for the bottom base.
Now we are going to create the top base - the cover of the assembly - based on reference geometry from the bottom base.
We will first create sketches, then create faces using the sketches. To make things easier, we will first create half of the top base and then copy it by using the Mirror option.
Step 2 - Create Sketches
Enter the Sketcher, using the top face of the base as the sketching plane.
Add as reference geometry the circle and three edges indicated below. How?
Click the Add Reference icon 
. Select the entities, and exit when finished.
Create one line and two arcs. Align vertically with the center of the circle. For the arcs, use the Tangent constraint.
How?
Creating a tangent arc:
1. Select the first point using the On Curve constraint.
2. Select the second point the same way.
3. When sizing the radius, the curve turns dashed blue when tangent.
Create the lower arc the same way.
Exit the Sketcher.
We now want to create another sketch, on a vertical plane passing halfway through the plate.
Create this vertical plane.
There are several ways to create this plane:
Normal:
First select a plane to which the new plane will be normal.
Then select two points (or a line) that lies on the new plane.
Defined By:
Pick three points that define the plane (in this case, three midpoints).
Parallel:
First select a plane to which the new plane will be parallel.
Change By Offset to By Point, and select a point that lies on the new plane.
Enter the Sketcher using this plane, and add the midpoints of the two long edges as reference geometry.
Now switch to right view and create two vertical lines.
Change these vertical lines into construction lines. How?
In Select mode, select the two lines. Click the Change Construction Lines icon 
.
Now create three arcs. Make the two outer arcs tangent to the constructions lines.
How?
Making arcs tangent to the construction lines:
Create the two endpoints using the default Pt option.
From the popup menu pick Tangent, then select the construction line.
Assign the dimensions shown below. (The 84.5 and 50.0 dimensions are between the center points of the right and center arcs.)
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