Skateboard. Hanger. in the Feature Manager and click Sketch. (S) on the Sketch. Line

Transcription

1 Chapter 3 Skateboard Hanger A. Sketch 1. Step 1. Click File Menu > New, click Part Metric and OK. Step 2. Click Right Plane from the Content toolbar, Fig. 1. in the Feature Manager and click Sketch Step 3. Click Centerline (S) in the Line flyout on the Sketch toolbar. Step 4. Draw the three construction lines as shown in Fig. 2. Double click centerline to end chain. Origin Fig. 1 Step 5. Click Smart Dimension toolbar. (S) on the Sketch Step 6. Add dimensions as shown in Fig. 3. Fig. 2 Step 7. Click Line (L) on the Sketch toolbar. Step 8. Draw line at slight angle below end of left construction line, Fig. 4. Step 9. Right click drawing and click Select from menu to unselect Line tool. Step 10. Ctrl click line and bottom endpoint of left construction line to select both. Release Ctrl key and click Make Midpoint on the Content menu, Fig. 5. Step 11. Ctrl click line and construction line to select both. Release Ctrl key and click Make Perpendicular menu, Fig. 6. Ctrl click line and endpoint on the Content Line Ctrl click line and construction line Fig. 3 Fig. 4 Fig. 5 Fig. 6 SolidWorks 12 HANGER SKATEBOARD Page 3-1 Cudacountry.net Tech Ed cudacountry@hotmail.com 9/19/12

2 B. Save as "HANGER". Step 1. Click File Menu > Save As. 2. Click endpoint Step 2. Key-in HANGER for the filename and press ENTER. C. Sketch 1 Part 2. Step 1. Click Centerpoint Arc the Arc flyout toolbar. (S) in on the Sketch Step 2. Click the Origin to start the arc. Move cursor up vertically from the Origin and click to place the first end point. Then move cursor clockwise past 180 degrees and click to place the second end point, Fig Start at Origin 3. Drag around and click to end arc Fig. 7 Ctrl click arc endpoint and Origin Step 3. Right click drawing and click Select from menu to unselect Arc tool. Step 4. Ctrl click top endpoint of arc and Origin to select both. Release Ctrl key and click Make Vertical Content menu, Fig. 8. on the Fig. 8 Step 5. Click Smart Dimension (S) on the Sketch toolbar. Step 6. Dimension line 35 and arc 9 as shown in Fig. 9. Step 7. Click Line toolbar. (L) on the Sketch Fig. 9 Step 8. Draw line tangent from arc to right endpoint of line, Fig. 10. Fig. 10 SolidWorks 12 HANGER SKATEBOARD Page 3-2

3 Step 9. Right click drawing and click Select from menu to unselect Line tool. Step 10. Ctrl click new line and arc. Release Ctrl key and click Make Tangent on the Content menu, Fig. 11. Step 11. Click Trim Entities the Sketch toolbar. on Step 12. In the Property Manger select Ctrl click arc and line Fig. 11 Corner, Fig. 12. Click arc at Position 1 and line at Position 2 to trim arc, Fig Step 13. Click Spline Sketch toolbar. (S) on the 2 Step 14. Draw 2 point spline between top endpoint of arc and top endpoint of first line, Fig. 14. Press Escape to end spline. Step 15. Add Tangent relation between the top end of spline and arc. Ctrl click spline and arc to select both. Release Ctrl key Fig. 12 Spline Fig. 13 and click Make Tangent Content menu, Fig. 15. on the Fig. 14 Ctrl click line and arc Fig. 15 SolidWorks 12 HANGER SKATEBOARD Page 3-3

4 Step 16. Click Sketch Fillet Sketch toolbar. (S) on the Step 17. In the Property Manager set: Radius 2, Fig. 16 click endpoints of first line at spline and at line, Fig. 17 click Yes to messages click OK twice. Fig. 17 Step 18. Click Smart Dimension toolbar. (S) on the Sketch Step 19. Dimension line 27 as shown in Fig. 18. Fig. 16 Step 20. Right click drawing and click Select from menu to unselect Smart Dimension. Step 21. Right click spline and click Display Control Polygon from menu, Fig. 19. Step 22. Click spline to select it. Click the top left Spline Control Point of spline (3rd from left), Fig. 19. In the Spline Polygon Property Manger set: X -24 Y 8 click OK, Fig. 20. Control Point Fig. 18 Right click Spline Step 23. Click Exit Sketch the Sketch toolbar. on Fig. 19 Step 24. Save. Use Ctrl-S. Fig. 20 SolidWorks 12 HANGER SKATEBOARD Page 3-4

5 D. Create Two Planes. Step 1. Click Isometric on the Standard Views toolbar. Step 2. Click Right Plane in the Feature Manager, Fig. 21. Step 3. Ctrl drag Right plane in drawing area to RIGHT and release, Fig. 22. Step 4. In the Plane Property Manager set: Distance 64 press ENTER key on keyboard uncheck Flip, Fig. 23. Hold down Ctrl drag Right plane Fig. 21 The new Plane should be to the RIGHT of the Right Plane, if it is not, check Flip Drag in this direction set distance to 64 click OK. Step 5. Again, click Right Plane in the Feature Manager. Step 6. Ctrl drag Right plane in drawing area to LEFT and release, Fig. 24. Fig. 22 Fig. 23 Step 7. In the Plane Property Manager set: Distance 64 press ENTER key on keyboard check Flip, Fig. 23. The new Plane should be to the LEFT of the Right Plane, if it is not, uncheck Flip click OK. Hold down Ctrl drag Right plane Fig. 25 Drag in this direction set distance to 64 Fig. 24 SolidWorks 12 HANGER SKATEBOARD Page 3-5

6 E. Sketch in Plane1. Step 1. Click Plane1 in the Feature Manager and click Sketch on the Content menu, Fig. 26. Step 2. Click Normal To on the Views toolbar (Ctrl-8). Step 3. Click Circle (S) on the Sketch toolbar. Origin Fig. 26 Step 4. Draw circle at Origin, Fig. 27. Step 5. Click Smart Dimension (S) on the Sketch toolbar. Step 6. Dimension diameter 18, Fig. 27. Step 7. Click Exit Sketch Sketch toolbar. on the Fig. 27 F. Copy Sketch2 to Plane2. Step 1. Click Isometric toolbar. on the Standard Views Step 2. Click the Sketch2 in the Feature Manager, Fig. 28 and copy. Use Ctrl-C to copy sketch. Step 3. Click the Plane2 in the Feature Manager, Fig. 29 and paste sketch. Use Ctrl-V to paste sketch, Fig. 30. Step 4. Save. Use Ctrl-S. Fig. 28 Fig. 29 SolidWorks 12 HANGER SKATEBOARD Page 3-6

7 G. Loft Boss/Base. Step 1. Click Features Step 2. Click Lofted Boss/Base on the Command Manager toolbar. on the Features toolbar. Step 3. In the Loft Property Manager: under Profiles click the same position on the three sketches, Fig. 30: Sketch3 Sketch1 Sketch2 expand Start/End Constraints under Start/End Constraints: set Start constraint: Normal to Profile set Start Tangent Length: 1.3 Fig. 31 set End constraint: Normal to Profile set Start Tangent Length: 1.3 Click Front on the Standard Views toolbar (Ctrl-8) Fig. 30 Right click the loft and click Zebra stripes preview from menu to check the alignment of the profiles If necessary, reposition the connector points of profiles to align loft Fig. 32 Right click the loft again, click Zebra stripes preview from menu to turn off stripes Click OK Manager. in the Property Fig. 33 Step 4. Click Isometric on the Standard Views toolbar. Step 5. Save. Use Ctrl-S. SolidWorks 12 HANGER SKATEBOARD Page 3-7

8 H. Create Plane3 for Kingpin Hole. Step 1. Expand Loft1 (click +) in Feature Manager, click Sketch1 and Show Fig. 34. on the Content menu, Step 2. Click Loft1 in Feature Manager and click Hide on the Content menu, Fig. 35. Step 3. Click Reference Geometry on the Features toolbar and Plane from the menu. Fig. 34 Fig. 35 Step 4. In the Plane Property Manager: under First Reference click front construction line click Perpendicular, Fig. 36 under Second Reference click bottom endpoint of front construction line, Fig. 37 and click OK I. King Pin Hole. Fig. 36 Fig. 37 Construction line Endpoint Step 1. Click Hole Wizard on the Features toolbar. Step 2. In the Property Manager, on the Type tab and set: under Hole Type: click Counterbore, Fig. 38 under Standard: select ANSI Metric under Hole Specification: check Show custom sizing and set: Through Hole Diameter 13 Counterbore Diameter 26 Counterbore Depth 2.7 click Positions tab at the top of the Property Manager. SolidWorks 12 HANGER SKATEBOARD Page 3-8 Fig. 38

9 Step 3. Click Plane3 in the drawing area as face to where you want to place the hole, Fig. 39. Step 4. Click the Origin to place point of hole at Origin, Fig. 40. Step 5. Click OK in the Hole Wizard Property Manager. Step 6. You can click Loft1 and click Show Plane 3 Fig. 39 on the Content menu to see hole in loft, but we will keep Loft hidden to better illustrate the next two planes and sketches. Fig. 40 J. Create Plane4 and Plane5 for Lofted Cut. Step 1. Ctrl drag Plane3 in drawing area, drag up and release, Fig. 41. Step 2. In the Plane Property Manager set: Hold down Ctrl Distance 5 drag Plane3 press ENTER key on keyboard check Flip, Fig. 23 click OK. Drag in this direction set distance to 5 Step 3. Ctrl drag Plane4 in drawing area up and release, Fig. 43. Step 4. In the Plane Property Manager set: Fig. 41 Fig. 42 Distance 25 press ENTER key check Flip, Fig. 23 click OK. Drag up set distance to 25 Hold down Ctrl drag Plane4 Fig. 43 SolidWorks 12 HANGER SKATEBOARD Page 3-9 Fig. 42

10 K. Create Circle in Plane4 for Lofted Cut. Step 1. Click Plane4 in the Feature Manager and click Sketch on the Content menu, Fig. 45. Step 2. Click Circle (S) on the Sketch toolbar. Step 3. Draw circle, Fig. 46. Step 4. Right click drawing and click Select from menu to unselect Circle tool. Step 5. Ctrl click centerpoint of circle and front construction line. Release Ctrl key and click Make Pierce on the Content menu, Fig. 47. Ctrl click centerpoint and construction line Fig. 45 Step 6. Click Smart Dimension (S) on the Sketch toolbar. Fig. 46 Fig. 47 Step 7. Dimension diameter 26, Fig. 48. Step 8. Click Exit Sketch on the Sketch toolbar. Fig. 48 L. Create Ellipse in Plane5 for Lofted Cut. Step 1. Click Plane5 in the Feature Manager and click Sketch on the Content menu, Fig. 49. Step 2. Click Normal To on the Standard Views toolbar. (Ctrl-8) Step 3. Click Ellipse on the Sketch toolbar. Fig. 49 SolidWorks 12 HANGER SKATEBOARD Page 3-10

11 Step 4. Draw ellipse at centerpoint of circle as shown in Fig. 50. To draw ellipse, move Major axis cursor up from Origin along Sketch1, start ellipse when center of circle highlights. Drag out and click to place major axis. Drag up and click again to set the minor axis. Minor axis Centerpoint Step 5. Click Smart Dimension Sketch toolbar. (S) on the Step 6. Dimension ellipse as shown in Fig. 51. To Smart dimension, click the major axis points, then move the cursor up off the sketch and click. Key-in 60 for major diameter dimension and press ENTER. Dimension minor diameter Fig. 50 Step 7. Click Exit Sketch on the Sketch toolbar. M. Lofted Cut Kingpin Nut Boss. Step 1. Click Isometric on the Standard Views toolbar. Fig. 51 Step 2. Click Loft1 in Feature Manager and click Show menu, Fig. 52. on the Content Step 3. Click Features Step 4. Click Lofted Cut on the Command Manager toolbar. on the Features toolbar. Fig. 52 SolidWorks 12 HANGER SKATEBOARD Page 3-11

12 Step 5. In the Loft Property Manager, under Profiles: Fig. 53 click the same position on the two sketches, Fig. 54: Sketch6 Sketch7 Click Front on the Standard Views toolbar (Ctrl-8) and check connector points to align loft the connec- align loft If necessary, reposition tor points of profiles to If necessary, right click the loft and click Zebra stripes preview from menu to check the alignment of the profiles Fig. 54 Fig. 53 Click OK Manager. in the Property Fig. 55 Step 6. Save. Use Ctrl-S. N. Hide Planes. Step 1. Hide Planes 1-5. To hide planes, Ctrl click planes 1-5 in Feature Manager. Release Ctrl and click Hide Content menu, Fig. 57. on the Fig. 56 SolidWorks 12 HANGER SKATEBOARD Page 3-12 Fig. 57

13 O. Fillet Edges. Step 1. Rotate view as shown in Fig. 59 to view underside kingpin counterbore, hold down middle mouse button (wheel) and drag to rotate view. R.25 Fig. 59 Step 2. Click Fillet Features toolbar. on the Step 3. In the Fillet Property Manager: select FilletXpert, Fig. 60 Radius.25 Fig. 60 R 1.7 Fig. 62 Click both edges of the bottom kingpin counterbore, Fig. 59. Click Apply Step 4. Click Isometric on the Standard Views toolbar. Fig. 61 R 1.2 R 2 Fig. 63 Radius 1.7, Fig. 61 Click the bottom inside edge of lofted cut, Fig. 62. Click Apply Fig. 61 Fig. 64 R 2 Continue and add Fillets: Top edge of lofted cut, Radius 1.2, Fig. 63. Both end edges of loft, Radius 2, Fig. 64. Click OK. Step 5. Save. Use Ctrl-S. SolidWorks 12 HANGER SKATEBOARD Page 3-13

14 P. Axle Hole. Step 1. Click Right Plane in the Feature Manager and click Sketch from the Content toolbar, Fig. 65. Step 2. Click Normal To on the Standard Views toolbar. (Ctrl-8) Step 3. Click Circle on the Sketch toolbar. Step 4. Draw a circle starting at the Origin, Fig. 66. Step 5. Click Smart Dimension on the Sketch toolbar. Fig. 65 Step 6. Dimension circle diameter 8 as shown in Fig. 66. Step 7. Click Features toolbar. on the Command Manager Step 8. Click Extruded Cut on the Features toolbar. Fig. 66 Origin Step 9. Click Isometric on the Standard Views toolbar. Step 10. In the Property Manager set: End Condition to Mid Plane Depth 128 click OK Fig. 68. Step 11. Save. Use Ctrl-S., Fig. 67 and Fig. 67 Fig. 68 SolidWorks 12 HANGER SKATEBOARD Page 3-14

15 Q. Create Plane6 for Pivot Pin. Step 1. Click Reference Geometry from the menu. on the Features toolbar and Plane Step 2. In the Plane Property Manager: under First Reference click back construction line in Sketch1, Fig. 69 Click Perpendicular, Fig. 70 under Second Reference click Origin, Fig. 69 and click OK. Fig. 69 Fig. 70 R. Create Circle in Plane6 for Pivot Pin. Step 1. Click Plane6 in the Feature Manager and click Sketch on the Content menu, Fig. 71. Step 2. Click Normal To Step 3. Click Circle on the Views toolbar (Ctrl-8). (S) on the Sketch toolbar. Step 4. Draw a circle starting at the Origin, Fig. 72. Step 5. Click Smart Dimension Step 6. Dimension diameter 11.5, Fig. 73. (S) on the Sketch toolbar. Fig. 71 Step 7. Click Features on the Command Manager toolbar. Step 8. Click Extruded Boss/Base on the Features toolbar. Fig. 72 Origin Step 9. Click Right on the Standard Views toolbar. (Ctrl-4) SolidWorks 12 HANGER SKATEBOARD Page 3-15

16 Step 10. In the Property Manager set: under From Start Condition Offset Offset Value 5 under Direction 1 Depth 34 click Draft On and 2 degrees (inward) click OK, Fig. 73 and Fig. 74. Fig. 73 Fig. 74 S. Create Sketch for Plane7. Step 1. Click Front Plane in the Feature Manager and click Sketch from the Content toolbar, Fig. 75. Step 2. Click Front Step 3. Click Line on the Standard Views toolbar. (Ctrl-1) (L) on the Sketch toolbar. Step 4. Starting from the Origin draw line out to the right, Fig. 76. Step 5. Click Exit Sketch on the Sketch toolbar. Fig. 75 Origin Line Fig. 76 SolidWorks 12 HANGER SKATEBOARD Page 3-16

17 T. Create Plane7 for Rib. Step 1. Rotate view as shown in Fig. 77, hold down middle mouse button (wheel) and drag to rotate view. Step 2. Click Reference Geometry from the menu. on the Features toolbar and Plane Step 3. In the Plane Property Manager: under First Reference click new line in Sketch10, Fig. 77 under Second Reference click bottom face of pivot pin, Fig. 77 and click OK Line Fig. 77 Face Fig. 78 U. Sketch in Plane7 for Rib. Step 1. Click Sketch10 in Feature Manager click Hide Step 2. Click Plane7 on the Content menu, Fig. 79. in the Feature Manager and click Sketch on the Content menu, Fig. 80. Step 3. Click Normal To (Ctrl-8). on the Views toolbar Step 4. Click Spline (S) on the Sketch toolbar. Step 5. Draw 2 point spline between underside of hanger and pivot pin, Fig. 81. To draw spline, move cursor to bottom edge under hanger and when edge turns red, click for first spline point. For 2nd spline point, move cursor to edge of pivot pin, when edge turns red, click. Press Escape to end spline. Spline Fig. 79 Fig. 80 Fig. 81 SolidWorks 12 HANGER SKATEBOARD Page 3-17

18 Step 6. Click Smart Dimension (S) on the Sketch toolbar. Origin Step 7. Dimension spline point to Origin 26 and 4.5 to edge of hanger as shown Fig. 82. Step 8. Right click drawing and click Select from menu to unselect Smart Dimension. Step 9. Click the spline to display the Circular Spline handles, Fig. 83. Step 10. Grab the Circular Spline handle of spline point at pivot pin, pull up slightly to adjust spline, Fig. 83. Pull Circular spline handle Fig. 82 Fig. 83 Step 11. In the Spline Property Manager: under Parameters, Fig. 84 check Tangent driving set Tangent Radial Direction -42.8º Control Point Step 12. Click Smart Dimension (S) on the Sketch toolbar. Step 13. Dimension Tangent Weighting1 30, Fig. 83. To dimension Tangent Weighting, click the Circular Spline handle, then move the cursor out away from spline and click. Key-in 30 and press ENTER. Step 14. Click Features on the Command Manager toolbar. Step 15. Click Rib on the Features toolbar. Fig. 84 Step 16. In the Rib Property Manager set: Both sides, Fig. 85 Rib thickness 3 check Flip material side click Draft On 6 degrees uncheck Draft outward click OK, Fig. 86. Fig. 85 Fig. 86 SolidWorks 12 HANGER SKATEBOARD Page 3-18

19 V. Mirror Rib. Step 1. Expand Loft1 (click +) in Feature Manager, click Sketch1 and click Hide menu, Fig. 87. on the Content Step 2. Also, Hide Planes 6 and 7, Fig. 87. Step 3. Ctrl click Right Plane and Rib1 feature in the Feature Manager to select both, Fig. 88. Step 4. Click Mirror on the Features toolbar. Step 5. Click OK Mirror Property Manager, Fig. 89 and Fig. 90. Step 6. Save. Use Ctrl-S. W. Fillet Edges. Step 1. Rotate view as shown in Fig. 90, hold down middle mouse button (wheel) and drag. Fig. 90 Fig. 87 Fig. 88 Step 2. Click Fillet on the Features toolbar. Step 3. In the Fillet Property Manager: select FilletXpert, Fig. 91 Radius 1 Fig. 89 click the bottom edges of ribs, Fig. 92 click Apply R 1 R 1 Fig. 92 Fig. 91 SolidWorks 12 HANGER SKATEBOARD Page 3-19

20 Radius 3.5 Click other edges of ribs on both sides, Fig. 93. R 3.5 Continue and add Fillets: Top edge of pivot pin on both sides, Radius 5, Fig. 94. Fig. 93 R 3.5 Bottom face of pivot pin, Radius 4.5, Fig. 95. click OK Step 4. Save. Use Ctrl-S. Fig. 94 R 5 Fig. 95 R 4.5 SolidWorks 12 HANGER SKATEBOARD Page 3-20

21 X. Appearance. Step 1. Click Render Tools on the Command Manager toolbar. Step 2. Click Preview Window or Integrated Preview on the Render Tools toolbar. Step 3. Click Edit Appearance on the Render Tools toolbar. Step 4. In the Appearances Task pane, expand Metal, click Aluminum and in the lower pane select cast aluminum, Fig. 97. Step 5. Back over in the Appearances Property Manager, click Advanced button, Fig. 97 under Color: set RGB values to: R 215 G 234 B 255 Fig. 96 Fig. 97 Fig. 98 SolidWorks 12 HANGER SKATEBOARD Page 3-21

22 Step 6. Click the Mapping tab, Fig. 99 under Mapping Mapping Type Automatic under Size/Orientation Width 60 press Tab key Fig. 100 Fig. 100 Fig. 99 Step 7. Click Surface Finish tab, Fig. 101 under PhotoView Surface Finish check Bump Mapping Bump Strength.1 Fig. 102 click OK. Step 8. Save. Use Ctrl-S. Fig. 101 Fig. 102 SolidWorks 12 HANGER SKATEBOARD Page 3-22