Chapter 1 A. New Part. Step 1. Click File Menu > New. Simple Machines Body Step 2. Click Part from the list and click OK, Fig. 1. B. Sketch Construction Rectangle. Step 1. Click Right Plane in the Feature Manager and click Sketch from the Content toolbar, Fig. 2. Step 2. Click Rectangle (S) on the Sketch toolbar. Fig. 1 Step 3. Draw a rectangle starting at the Origin and before you move the cursor away from the rectangle, right click a line and click Construction Geometry on the Content menu, Fig. 3. Step 4. Click Smart Dimension (S) on the Sketch toolbar. Fig. 2 Step 5. Add dimensions as shown in Fig. 4. To Smart dimension, click the line then move the cursor out away from the line and click. Key-in the dimension and press ENTER. Arrange the dimensions as shown in Fig. 4. Step 6. Click Zoom to Fit toolbar. C. Save as "BODY". Step 1. Click File Menu > Save As. (F) on the View Step 2. Key-in BODY for filename and press ENTER. Origin Fig. 3 Fig. 4 SolidWorks 12 BODY SIMPLE MACHINES Page 1-1 Cudacountry.net Tech Ed http://www.cudacountry.net email:cudacountry@hotmail.com 1/6/12
D. Lines. Step 1. Click Line toolbar. (L) on the Sketch Step 2. Draw the 8 lines in Fig. 5. Step 3. Click Smart Dimension (S) on the Sketch toolbar. Step 4. Add dimensions as shown in Fig. 6. To Smart dimension an angle, click both lines, then move the cursor inside the angle and click. Key-in angle for the dimension and press ENTER. Add the other dimensions. Fig. 5 E. Sketch Fillet. Step 1. Click Sketch Fillet Sketch toolbar. on the Fig. 6 Step 2. In the Sketch Fillet Property Manager set: Radius to.2, Fig. 7 click the 5 corners in Fig. 8, click OK twice, Fig. 9. Fig. 8 Fig. 7 Fig. 9 SolidWorks 12 BODY SIMPLE MACHINES Page 1-2
F. Extrude. Step 1. Click Features on the Command Manager toolbar. Step 2. Click Extruded Boss/Base on the Features toolbar. Step 3. In the Property Manager set: under Direction 1, Fig. 10 End Condition to Mid Plane Depth to 1.5 click OK, Fig. 11. Step 4. Save. Use Ctrl-S. G. Axle Holes. Step 1. Click the side face of Truck and click Sketch menu, Fig. 11. on the Content Fig. 10 Fig. 11 Side face Step 2. Click Normal To Step 3. Click Circle on the View toolbar. (Ctrl-8) (S) on the Sketch toolbar. Step 4. Draw two circles for the axle holes, Fig. 12. Step 5. Click Smart Dimension (S) on the Sketch toolbar. Step 6. Add dimensions as shown in Fig. 13. To Smart dimension circle, click the circle then move the cursor out away from circle and click. Key-in.15 for diameter and press ENTER. To add other dimensions, click circle and edge of body, move cursor just off of body and click. Key in dimension and press ENTER. Arrange the dimensions as shown in Fig. 13. Fig. 12 Fig. 13 SolidWorks 12 BODY SIMPLE MACHINES Page 1-3
Step 7. Click Trimetric on the Standard Views toolbar. Step 8. Click Features Step 9. Click Extruded Cut on the Command Manager toolbar. on the Features toolbar. Top face truck bed Step 10. In the Property Manager set: under Direction 1 End Condition to Through All click OK, Fig. 14 and Fig. 15. Step 11. Save. Use Ctrl-S. H. Cut Bed. Step 1. Click the top face of Truck bed and click Sketch on the Content menu, Fig. 15. Fig. 14 Fig. 15 Step 2. Click Normal To on the Views toolbar (Ctrl-8). Step 3. Click Offset Entities on the Sketch toolbar. Step 4. In the Offset Entities Property Manager set: Distance to.05 Fig. 16 check Reverse top face of Truck bed should be selected, Fig. 17 The yellow offset should be inside the Truck bed, Fig. 17. If it is not, uncheck Reverse. Click OK. Step 5. Click Trimetric on the Standard Views toolbar. Fig. 16 Fig. 17 Step 6. Click Features on the Command Manager toolbar. SolidWorks 12 BODY SIMPLE MACHINES Page 1-4
Step 7. Click Extruded Cut on the Features toolbar. Step 8. In the Property Manager set: under Direction 1, Fig. 18 Depth to.75 click OK, Fig. 19. Step 9. Save. Use Ctrl-S. I. Side Windows. Step 1. Click the side face of Truck and click Sketch menu, Fig. 19. on the Content Fig. 18 Fig. 19 Side face Step 2. Click Normal To on the Views toolbar (Ctrl-8). Step 3. Press Escape key to unselect the face. Step 4. Click Offset Entities on the Sketch toolbar. Step 5. In the Offset Entities Property Manager set: Distance to.1 Fig. 20 check Reverse Fig. 20 click the 5 edges around the Truck cab, Fig. 21. The yellow offset should be inside the cab, Fig. 21. If it is not, uncheck Reverse. Click OK. Fig. 21 Step 6. Click Line (L) on the Sketch toolbar. Step 7. Draw Line across bottom endpoints, Fig. 22. Step 8. Click Trimetric Views toolbar. on the Standard Fig. 22 SolidWorks 12 BODY SIMPLE MACHINES Page 1-5
Step 9. Click Features on the Command Manager toolbar. Step 10. Click Extruded Cut Features toolbar. on the Step 11. In the Property Manager set: under Direction 1, Fig. 23 Depth to.05 click OK, Fig. 24. Step 12. Save. Use Ctrl-S. Fig. 23 Fig. 24 J. Mirror Side Window. Step 1. Select Right Plane and Cut-Extrude3 (side window) in Feature Manager, Fig. 25. To select, click Right Plane in Feature Manager. Hold down Ctrl key and click Cut-Extrude3. Step 2. Click Mirror on the Features toolbar. Step 3. In the Mirror Property Manager click OK, Fig. 27. Fig. 25 Step 4. Save. Use Ctrl-S. K. Windshield. Step 1. Rotate view to view right side window, Fig. 28. Hold the middle mouse button (wheel) and rotate wheel around to view. Step 2. Click the face of windshield and click Sketch menu, Fig. 28. on the Content Fig. 26 Fig. 27 Windshield face Step 3. Click Normal To (Ctrl-8). on the Views toolbar Fig. 28 SolidWorks 12 BODY SIMPLE MACHINES Page 1-6
Step 4. Click Offset Entities on the Sketch toolbar. Step 5. In the Offset Entities Property Manager set: Distance to.07 Fig. 29 check Reverse the face of front windshield should be selected, Fig. 30. The yellow offset should be inside the Truck, Fig. 30. If it is not, uncheck Reverse. Click OK. Fig. 29 Fig. 30 Step 6. Click Features on the Command Manager toolbar. on the Stan- Step 7. Click Extruded Cut Features toolbar. Step 8. Click Trimetric dard Views toolbar. on the Step 9. In the Property Manager set: under Direction 1, Fig. 31 Depth to.05 click OK, Fig. 32. Fig. 31 Fig. 32 Step 10. Save. Use Ctrl-S. L. Mate References. Step 1. Click Right Plane in the Feature Manager to select Plane, Fig. 33. Step 2. Click Reference Geometry Reference from the menu. on the Features toolbar and Mate Fig. 33 SolidWorks 12 BODY SIMPLE MACHINES Page 1-7
Step 3. In the Mate Reference Manager: under Primary Reference Entity, Fig. 34 set Mate Reference Type under Secondary Reference Entity click in Entity box and click inside cylindrical face of front axle hole, Fig. 35 click OK. to Coincident Step 4. Click Right Plane in the Feature Manager to select Plane, Fig. 36. Step 5. Click Reference Geometry Reference from the menu. Face Fig. 35 on the Features toolbar and Mate Fig. 34 Step 6. In the Mate Reference Manager: under Primary Reference Entity, Fig. 37 set Mate Reference Type under Secondary Reference Entity click in Entity box and click inside cylindrical face of rear axle hole, Fig. 38 click OK. Step 7. Save. Use Ctrl-S. to Coincident Face Fig. 36 Fig. 38 Fig. 37 SolidWorks 12 BODY SIMPLE MACHINES Page 1-8
M. Material Pine. Step 1. Right click Material Material, Fig. 39. in the Feature Manager and click Edit Step 2. Expand Woods (click the +) in the material tree and click Pine, Fig. 40. Click Apply and Close, Fig. 41. Step 3. Save. Use Ctrl-S. N. Appearance. Step 1. Click the Body to select the part, click Appearances Callout on the Content menu and click BODY, Fig. 41. Fig. 39 Fig. 40 Click part Fig. 41 SolidWorks 12 BODY SIMPLE MACHINES Page 1-9
Step 2. In the Appearances Task pane, expand Painted, click Car and in the lower pane select white, Fig. 42. Step 3. In the Appearances Property Manager, Fig. 43 under Color: set RGB values to: R 79 G 149 B 255 click Keep Visible and OK, Fig. 43. The Push Pin on allows selection of another appearance for windows. Fig. 42 Fig. 44 Fig. 43 SolidWorks 12 BODY SIMPLE MACHINES Page 1-10
Step 4. In the Appearances Property Manager, under Selected Geometry click Select Faces, Fig. 45 click window and windshield, Fig. 46. Then rotate view to select right side window, hold down middle mouse button (wheel) and drag to rotate view, Fig. 47. Click Advanced button at top of Property Manager, Fig. 48 Fig. 46 click Illumination tab, Fig. 48 set Transparency amount.50, Fig. 48 click OK and click Cancel. Step 5. Save. Use Ctrl-S. Fig. 47 Fig. 45 Fig. 49 SolidWorks 12 BODY SIMPLE MACHINES Page 1-11 Fig. 48