F1 Car. Wheel. in the Feature Manager and click Sketch on the Context toolbar, Fig. 1. (S) on the
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1 Chapter 3 F1 Car Wheel A. Sketch Lines. Step 1. Click File Menu > New, click Part Metric and OK. Step 2. Click Front Plane in the Feature Manager and click Sketch on the Context toolbar, Fig. 1. Step 3. Click Line (L) on the Sketch toolbar. Step 4. Draw lines starting at the Origin, Fig. 2. Use the inferencing line, the dotted line that appears when you draw the lines. Fig. 1 Step 5. Click Smart Dimension Sketch toolbar. (S) on the Step 6. Start dimensioning at the bottom line with 13, Fig. 3, then the 2.5 and continue around the sketch. Dimension the 9 from line to line and not to corners. Origin Step 7. Click Zoom to Fit (F) on the View toolbar. Fig. 2 B. Save as "WHEEL". Step 1. Click File Menu > Save As. Step 2. Key-in WHEEL for the filename and press ENTER. Dimension 9 from line to line Fig. 3 SOLIDWORKS 15 Wheel F1 CAR Page 3-1 Cudacountry.net Tech Ed cudacountry@hotmail.com 1/21/15
2 C. Offset Entities. Step 1. Click Offset Entities on the Sketch toolbar. Step 2. In the Offset Entities Property Manager set: under Parameters, Fig. 4 Distance 1.7 uncheck Select chain click 3 lines, Fig. 5 The yellow offset should be inside the original green geometry, Fig. 5. If it is not, uncheck Reverse. Step 3. Save. Use Ctrl-S. Fig. 4 Fig. 5 D. Lines for Hub and Cap Offset. Step 1. Click Line (L) on the Sketch toolbar. Step 2. Draw the 6 lines, Fig. 6. Use the automatic horizontal relation, cursor will change to yellow vertical horizontal icon as you draw up from Origin, Fig. 6. Be sure to cap offsets line at top left of sketch. Step 3. Click Smart Dimension Sketch toolbar. Step 4. Add dimensions, Fig. 7. Step 5. Save. Use Ctrl-S. (S) on the Fig. 6 Fig. 7 SOLIDWORKS 15 Wheel F1 CAR Page 3-2
3 E. Trim Corner. Step 1. Click Trim Entities toolbar. (S) on the Sketch Step 2. In the Trim Property Manger: select Corner, Fig. 8. Trim lines to extent Click both line, Fig. 9. Results shown in Fig. 10. Click OK done. when Fig. 9 F. Lines for Tire and Rim. Step 1. Zoom in around top right corner of the sketch, the tire surface, Fig. 10. To zoom, place the cursor over Fig. 8 the top right corner and spin the wheel on mouse back. While spinning the wheel keep cursor on area. Zoom Step 2. Click Line Step 3. Draw two lines, Fig. 11. (L) on the Sketch toolbar. Fig. 10 Step 4. Click Smart Dimension Sketch toolbar. (S) on the Step 5. Add dimensions, Fig. 12. Step 6. Save. Use Ctrl-S. Fig. 11 Fig. 12 SOLIDWORKS 15 Wheel F1 CAR Page 3-3
4 G. Trim. Step 1. Click Trim Entities (S) on the Sketch toolbar. Step 2. In the Trim Property Manger: select Trim to closest, Fig. 13. Trim way corner, Fig. 14. Results shown in Fig. 15. Click OK done. when H. Sketch Fillet. Step 1. Click Sketch Fillet on the Sketch toolbar. (S) Fig. 13 Fig. 14 Fig. 15 Step 2. In the Sketch Fillet Property Manager set: Radius.25, Fig. 16 click two corners, Fig. 17 click OK twice. Step 3. Save. Use Ctrl-S. I. Revolved Boss/Base. Step 1. Click Features on the Command Manager toolbar. Step 2. Click Revolved Boss/Base Fig. 16 Fig. 17 Fig. 18 on the Features toolbar. Step 3. In the Revolve Property Manger: for Axles of Revolution, Fig. 19 click bottom line, Fig. 20 Step 4. Save. Use Ctrl-S. Fig. 19 Fig. 20 SOLIDWORKS 15 Wheel F1 CAR Page 3-4
5 J. Fillet1. Step 1. Use Left arrow key on keyboard to rotate view to view inside edges of Wheel, Fig. 22. on the Fea- Step 2. Click Fillet tures toolbar. Step 3. In the Fillet Property Manager, select FilletXpert, Fig. 21 Radius 2 under Items To Fillet click both inside bottom edges, Fig. 22 K. Hole for Axle. Fig. 21 Step 1. Hold the middle mouse button (wheel) and rotate wheel around to view the back side, Fig. 23. Step 2. Click side face of the hub and click Sketch the Context toolbar, Fig. 23. on Hub Face Fig. 22 Step 3. Click Circle (S) on the Sketch toolbar. Step 4. Draw circle for hole at the Origin, Fig. 24. Step 5. Click Smart Dimension toolbar. Step 6. Dimension diameter 3.5, Fig. 24. (S) on the Sketch Fig. 23 Fig. 24 SOLIDWORKS 15 Wheel F1 CAR Page 3-5
6 Step 7. Click Features on the Command Manager toolbar. Step 8. Click Extruded Cut on the Features toolbar. Step 9. In the Property Manager set: under Direction 1, Fig. 25 Depth 10 Step 10. Save. Use Ctrl-S. Fig. 26 L. Extrude Bolt. Step 1. Click Right on the Standard Views toolbar. (Ctrl-4) Fig. 25 Step 2. Click flat face inside the wheel and click Sketch on the Context toolbar, Fig. 28. Step 3. Click Polygon on the Sketch toolbar. Step 4. Draw a polygon for the bolt directly above the Origin, Fig. 28. Use the inferencing line, the dotted line that appears when you draw. Face Fig. 27 Step 5. Click Smart Dimension toolbar. (S) on the Sketch Step 6. Add dimensions, Fig. 29. Fig. 28 Fig. 29 SOLIDWORKS 15 Wheel F1 CAR Page 3-6
7 Step 7. Click Features on the Command Manager toolbar. Step 8. Click Extruded Boss/Base on the Features toolbar. Step 9. Hold the middle mouse button (wheel) and rotate wheel slightly to see extrude, Fig. 31. Step 10. In the Property Manager set: under Direction 1, Fig. 30 Depth 1 Step 11. Save. Use Ctrl-S. M. Chamfer Bolt. Step 1. With the extruded bolt still selected, click Zoom to Selection (Q) on the View toolbar to zoom around the bolt. Use the Z key to zoom out. Fig. 30 Fig. 31 Face Step 2. Click Chamfer Features toolbar. on the Step 3. In the Property Manager set: under Chamfer Parameters, Fig. 32 click top face of extruded bolt, Fig. 33 Distance.15 Fig. 32 Fig. 33 Fig. 34 SOLIDWORKS 15 Wheel F1 CAR Page 3-7
8 N. Circular Pattern for Bolts. Step 4. Click Circular Pattern in the Linear Pattern flyout on the Features toolbar. Click the flyout arrow to select Circular Pattern. Step 5. In the Circular Pattern Property Manager set: under Parameters, Fig. 35 click in Pattern Axis box click cylindrical face hub, Fig. 36 Number of Instances 8 check Equal spacing under Feature and Faces click chamfer and extrude bolt, Fig. 36 O. Chamfer Hub. Use cylindrical face as Axis Select chamfer and extrude Fig. 36 Step 1. Click Chamfer Features toolbar. on the Step 2. In the Property Manager set: under Chamfer Parameters, Fig. 37 click front face of hub, Fig. 38 Distance.3 Fig. 35 Front face hub Fig. 38 Fig. 37 Fig. 39 SOLIDWORKS 15 Wheel F1 CAR Page 3-8
9 P. Mate Reference. Step 1. Click a cylindrical face to select it, Fig. 40. Face Step 2. Click Reference Geometry on the Surfaces toolbar and Plane from the menu. Step 3. In the Mate Reference Property Manager click OK, Fig. 41. Fig. 40 Q. Material POM Acetal Copolymer. Step 1. Right click Material in the Feature Manager and click Edit Material, Fig. 42. Fig. 41 Step 2. Expand Plastics in the material tree and select POM Acetal Copolymer, Fig. 43. Click Apply and Close. Fig. 42 Fig. 43 SOLIDWORKS 15 Wheel F1 CAR Page 3-9
10 R. Appearance. Step 1. Click Wheel to select part, click Appearances Callout, Fig. 44. on the Context toolbar and click WHEEL Click part Step 2. In the Appearances Task pane, expand Metal, click Chrome and in the lower pane select chromium plate, Fig. 45. Step 3. In the Appearances Property Manager, Click Keep Visible and OK, Fig. 46. Fig. 44 The Push Pin on allows selection of other materials (rubber for tires). Fig. 45 Fig. 46 SOLIDWORKS 15 Wheel F1 CAR Page 3-10
11 Step 4. In the Appearances Property Manager, under Selected Geometry click Select Faces, Fig. 47 click side face of tire and small fillet, Fig. 48. Face and fillet Fig. 49 Fig. 48 Step 5. Click Appearances, Scenes, and Decals tab to display the Task pane, Fig. 49. Step 6. In the Appearances Task pane, expand Rubber, Fig. 47 click Gloss and in the lower pane select glossy rubber, Fig. 49. Step 7. In the Appearances Property Manager, click Advanced button, Fig. 50 click Surface Finish tab under PhotoView Surface Finish Bump strength.1 Fig. 50 Fig. 51 SOLIDWORKS 15 Wheel F1 CAR Page 3-11
12 Step 8. Click cylindrical face of tire, Fig. 52. Step 9. Click Appearances, Scenes, and Decals tab to display the Task pane, Fig. 53. Step 10. In the Appearances Task pane, expand Rubber, click Texture and in the lower pane select tire tread, Fig. 53. Step 11. In the Appearances Property Manager, click Mapping tab, Fig. 54 Mapping type Cylindrical under Size/Orientation Width 8.5 click OK and click Cancel. Step 12. Save. Use Ctrl-S. Face Fig. 53 Fig. 52 Fig. 54 Fig. 55 SOLIDWORKS 15 Wheel F1 CAR Page 3-12
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