Activity 2.8: Create Gasket Substrate. Getting Started with CAD (SolidWorks)

In the CAD system, create a fully-defined and accurate cuboid shape from which the gasket will emerge. Try it. • Create and name a new part. Set the units to MMGS. • Use the sketch button (in the sketch command manager) to create a new CAD sketch. Deliberately choose the front plane to sketch on. • Use the corner rectangle command and draw a rectangle near but not on the origin. Notice the presence of 4 geometric relations. These tiny icons indicate geometric relations associated with the entity. Common entities are defined in Figure 2.6. If you do not see these tiny icons choose to show them by using the hide/show drop down menu. Figure 2.7 defines the meaning of these icons/relations. By choosing corner rectangle, the CAD system assumed that these relations were wanted. The drop down menu next to the corner rectangle provides other rectangle options that assume different relations. • Use the smart dimension command to define the size of the part. After clicking smart dimension, click on the lower horizontal line of the rectangle, then click again below that line. Change the value to 100 mm. • Click on the left vertical line, then click further to the left to dimension the rectangle height. Set the height to 150 mm. • Check the Fully-Defined/Under-Defined indicator. It reads Under Defined because only the size of the part has been defined. Its location in space is ambiguous. There are various ways to make the rectangle’s location unambiguous, but it is smart to use geometric relations. To specify relations, you must first exit the smart dimension command. You can do this by clicking the small green check mark on the left of the screen, or pressing ESC. • Fully locate the rectangle in space by choosing its bottom right point (hover on it then click), and while holding shift choose the origin. Release the shift key, and a menu will appear where you can add the geometric relation that will make the two selected points coincident. Notice that the sketch is now fully defined. Its size, shape, and location are fully specified. • Accept the sketch and return to the 3D geometry workspace. Accept by clicking the blue arrow in the top right of screen, or the exit sketch button in the command manager. • In the design tree, notice that there are now 5 geometric features in this part: front plane, top plane, right plane, origin, and the sketch you just made. • Use the sketch you just made to create a solid by clicking on the sketch name in the design tree (to indicate its selection, it will be highlighted when it is selected), then click the Extruded Boss/Base command, and change D1 from 10.00 mm to 5.00 mm. Finish the 3D operation (Extruded Boss/Base) by clicking the green check mark. • Assign PTFE (general), a plastic, as the material. • Save the part. This video accompanies the book Introduction to Mechanical Design with CAD by Christopher A. Mattson. It is a tutorial for Solidworks 2020-2021 edition.