We are almost done. We now create the mounting holes to secure the base. Make sure that the work plane in the middle of the part is visible.
-
Start a new sketch on the top face of the part. -
Start the Project Geometry command. Select the work plane in the middle of the part to project the work plane as a line to the current sketch. -
Place two points (Point, Center Point) vertically in-line with each other. -
Place a vertical constraint between the two points to align them. -
Add a 16-mm dimension from the center of the base to the upper center point. - Dimension the overall distance between the two points. Pick the two center points. Instead of adding a number for the overall distance, clear the value in the dialog box. Then, select the 16-mm dimension to add the dimension variable to the dialog box. Enter the multiplication operator *, and then the number 2. Note: The dimension variables in your sketch may differ from the numbers presented in the following image. If they do, it does not affect the exercise.
- Add a 33-mm dimension from the front edge of the part to one of the center points.
-
Finish the sketch. -
Start the Hole command. Place two through holes of 11 mm each on the center points. - Start a new sketch on the top face of the part.
-
Start the Line command. Create a line from the mid-point of the back edge of the base towards the middle of the part. - Add a dimension of 16 mm to the line.
- Finish the sketch.
In the remaining steps, we create a counterbore clearance hole for a hex head bolt from a look up table.
- Start the Hole command. Pick the endpoint of the line to specify the hole location.
- Select the counterbore hole with the clearance hole option as shown in the following image. The system determines the proper counterbore size for the fastener you specify.
- Select the fastener parameters listed in the image, and then click OK to create the hole.
- Save the file.
You have successfully completed this exercise!