Skateboard. Hanger. in the Feature Manager and click Sketch on the Context toolbar, Fig. 1. Fig. 2

Transcription

1 Chapter 3 Skateboard Hanger A. Sketch1 Lines. Step 1. Click File Menu > New, click Part Metric and OK. Step 2. Click Right Plane in the Feature Manager and click Sketch on the Context toolbar, Fig. 1. Step 3. Click Centerline in the Line flyout on the Sketch toolbar. Step 4. Draw the 2 construction lines starting Origin from Origin, Fig. 2. Fig. 1 Step 5. Click Smart Dimension (S) on the Sketch toolbar. Step 6. Add dimensions, Fig. 3. Fig. 2 Step 7. Click Midpoint Line in the Line flyout on the Sketch toolbar. Fig. 3 Step 8. Sketch a perpendicular midpoint line at bottom endpoint of construction line, Fig. 4. As you sketch use the icon to show perpendicular relation is added. B. Save as "HANGER". Step 1. Click File Menu > Save As. Step 2. Key-in HANGER for the filename and press ENTER. C. Sketch1 Arc and Spline. Step 1. Click Centerpoint Arc (S) in the Arc flyout on the Sketch toolbar. Fig. 4 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. 5. Fig. 5 SOLIDWORKS 15 Hanger SKATEBOARD Page 3-1 Cudacountry.net Tech Ed cudacountry@hotmail.com 5/20/15

2 Step 3. Right click graphics 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 toolbar, Fig. 6. on the Context Ctrl click endpoint and Origin Step 5. Click Smart Dimension on the Sketch toolbar. Step 6. Dimension arc radius 9, Fig. 7. (S) Fig. 6 Step 7. Click Line toolbar. (L) on the Sketch Step 8. Sketch line up from bottom endpoint of line tangent to arc right endpoint of line, Fig. 8. To sketch line, click bottom endpoint of line and click endpoint of arc, then click Make Tangent on the Context toolbar. Fig. 7 Step 9. Click Style Spline in the Spline flyout on the Sketch toolbar. Step 10. Draw a 3 control vertex point Spline between top endpoint of arc and top endpoint of line, Fig. 9. Start at top endpoint of arc for 1st control vertex point. Draw 2nd control vertex point to left. Click top endpoint of line for 3rd control vertex point. Press Escape to end spline. Fig Fig. 9 SOLIDWORKS 15 Hanger SKATEBOARD Page 3-2

3 Step 11. Click Sketch Fillet (S) on the Sketch toolbar. Step 12. In the Sketch Fillet Property Manager set: under Fillet Parameters, Fig. 10 Radius 2 click endpoints of first line at spline and at line and click Yes to messages, Fig. 11 click OK twice. Step 13. Click Smart Dimension (S) on the Sketch toolbar. Step 14. Dimension control vertex point and line, Fig. 12. Fig. 10 Fig. 11 Step 15. Right click graphics and click Select from menu to unselect Smart Dimension. Step 16. Click top control polygon segment and click Make Horizontal the Context toolbar, Fig. 13. on Step 17. Click Exit Sketch Step 18. Save. Use Ctrl-S. on the Sketch toolbar. Fig. 12 Fig. 13 Fig. 14 SOLIDWORKS 15 Hanger SKATEBOARD Page 3-3

4 D. Create Plane1 and Plane2. Step 1. Click Isometric on the Standard Views toolbar. (Ctrl-7) Step 2. Press Z key 2 or 3 times to zoom out. Step 3. Click Right Plane in the Feature Manager to display plane is graphics area, Fig. 15. Step 4. Ctrl drag Right plane in graphics area to right and release, Fig. 16. Hold down Ctrl drag Right plane Drag in this direction set distance 64 Fig. 15 Step 5. In the Plane Property Manager set: under First Reference, Fig. 17 Fig. 16 Distance 64 and press ENTER. The new plane should be to the right, Fig. 16. If in wrong direction, uncheck Flip offset. Fig. 17 Click Keep Visible and OK, Fig. 17. The Push Pin on allows adding another plane. Step 6. In the Plane Property Manager set: under First Reference, Fig. 18 click in First Reference box expand the flyout Feature Manager design tree in the top left corner of the graphics area and click Right Plane, Fig. 19 Distance 64 check Flip offset click OK and click Cancel. Fig. 19 Click Flip offset Fig. 18 Fig. 20 SOLIDWORKS 15 Hanger SKATEBOARD Page 3-4

5 E. Sketch in Plane1. Step 1. Click expand arrow at the top of the Feature Manager to expand the Display Pane, Fig. 21. Step 2. Hide Plane1 and Plane2, Fig. 21. To hide, in the Feature Manager Display Pane under Hide/Show column for Plane1 and Plane2 click Show to turn off show, Fig. 21 Step 3. Click Plane1 in the Feature Manager and click Sketch on the Context toolbar, Fig. 21. Step 4. Click Circle (S) on the Sketch toolbar. Step 5. Sketch circle at Origin, Fig. 22. Origin Step 6. Click Smart Dimension Sketch toolbar. Step 7. Dimension diameter 18, Fig. 22. (S) on the Fig. 22 Step 8. Click Exit Sketch on the Sketch toolbar. F. Copy Sketch2 into Plane2. Step 1. Click the Sketch2 in the Feature Manager and copy, Fig. 23. Use Ctrl-C to copy sketch. Step 2. Click the Plane2 in the Feature Manager and paste sketch, Fig. 24. Use Ctrl- V to paste sketch, Fig. 25. Step 3. Save. Use Ctrl-S. Fig. 23 Fig. 24 Fig. 25 SOLIDWORKS 15 Hanger SKATEBOARD Page 3-5

6 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, Fig. 26 click the same position on the three sketches, Fig. 27 Sketch3 Sketch1 Sketch2 expand Start/End Constraints under Start/End Constraints: Start constraint Normal to Profile Start Tangent Length: 1.3 End constraint Normal to Profile Start Tangent Length: 1.3 Click Front Expand Curvature display check Zebra stripes on the Standard Views toolbar (Ctrl-8) If necessary, reposition the connector points to align loft. Click OK. Fig. 26 Step 4. Save. Use Ctrl-S. Fig. 27 Fig. 28 Fig. 29 SOLIDWORKS 15 Hanger SKATEBOARD Page 3-6

7 H. Create Plane3 for Kingpin Hole. Step 1. Click Isometric on the Standard Views toolbar. (Ctrl-7) Step 2. Change Transparency of Loft1. To change transparency, move cursor to activate Loft1 row in the Feature Manager Display Pane and under Transparency column click Transparency to toggle transparency, Fig. 30. Step 3. Show Sketch1. To show, expand Loft1 in the Feature Manager under Hide/Show column for Sketch1 click Hide to turn off hide, Fig. 30. Fig. 30 Step 4. Click Reference Geometry from the menu. on the Features toolbar and Plane Step 5. In the Plane Property Manager: under First Reference, Fig. 31 click front construction line, Fig. 32 click Perpendicular under Second Reference click bottom endpoint of front construction line, Fig. 32 and click OK. Fig. 31 Construction line Fig. 32 Endpoint SOLIDWORKS 15 Hanger SKATEBOARD Page 3-7

8 I. King Pin Hole. Step 1. Click Hole Wizard on the Features toolbar. Step 2. In the Property Manager on the Type tab set: under Hole Type, Fig. 33 Counterbore 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 top of the Property Manager. Step 3. Click Plane3 as plane for hole, Fig. 34. Step 4. Click the Origin to place point of hole at Origin, Fig. 34. Fig. 33 Step 5. Click OK in the Hole Wizard Property Manager. Step 6. Hide Sketch1. To hide, click Sketch1 and Hide on the Context toolbar, Fig. 35. Fig. 34 Fig. 35 SOLIDWORKS 15 Hanger SKATEBOARD Page 3-8

9 J. Create Plane4 and Plane5 for Lofted Cut. Step 1. Ctrl drag Plane3 in graphics area up and release, Fig. 36. Step 2. In the Plane Property Manager set: under First Reference, Fig. 37 Distance 5 and press ENTER. The new plane should be above Plane3, Fig. 36. If in wrong direction, check Flip offset. Click Keep Visible and OK Pin plane., Fig. 37. The Push on allows adding another Step 3. In the Plane Property Manager set: under First Reference, Fig. 38 Plane4 should be selected Distance 25 press ENTER click OK and click Cancel. Drag up set distance 5 Ctrl drag Plane3 up Fig. 36 Fig. 37 Fig. 38 Fig. 39 SOLIDWORKS 15 Hanger SKATEBOARD Page 3-9

10 K. Create Sketch6 Circle in Plane4 for Lofted Cut. Step 1. Click Plane4 in the Feature Manager and click Sketch toolbar, Fig. 40. on the Context Step 2. Click Convert Entities Sketch toolbar. on the Step 3. In the Convert Entities Property Manager: under Entities to Convert, Fig. 41 click outside circular edge of counterbore, Fig. 42 Fig. 40 click OK twice. Note the converted edge in Plane4, Fig. 43. Fig. 41 Step 4. Click Exit Sketch on the Sketch toolbar. Edge Fig. 42 Converted edge in Plane4 Fig. 43 SOLIDWORKS 15 Hanger SKATEBOARD Page 3-10

11 L. Create Sketch7 Ellipse in Plane5 for Lofted Cut. Step 1. Click Plane5 in the Feature Manager and click Sketch on the Context toolbar, Fig. 44. Step 2. Click Normal To Step 3. Click Ellipse on the Standard Views toolbar. (Ctrl-8) on the Sketch toolbar. Step 4. Draw ellipse at Origin, Fig. 45. To draw ellipse, click Origin to start and move cursor up and click for minor axis. Drag out and click to place major axis. Fig. 44 Step 5. Right click graphics and click Select from menu to unselect Ellipse tool. Step 6. Ctrl click top axis point of ellipse and Origin to select both. Release Ctrl key and click Make Vertical on the Context toolbar, Fig. 46. Step 7. Click Smart Dimension (S) on the Sketch toolbar. Step 8. Dimension ellipse, Fig. 47. 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. 45 Fig. 46 Fig. 47 Origin Ctrl click axis point and Origin Step 9. Click Exit Sketch on the Sketch toolbar. SOLIDWORKS 15 Hanger SKATEBOARD Page 3-11

12 M. Lofted Cut Kingpin Nut Boss. Step 1. Click Isometric on the Standard Views toolbar. (Ctrl-7) Step 2. Click Features Step 3. Click Lofted Cut on the Command Manager toolbar. on the Features toolbar. Step 4. In the Loft Property Manager set: under Profile, Fig. 48 click the same position on the two sketches, Fig. 49 Sketch6 Sketch7 Click Front on the Standard Views toolbar (Ctrl-8) and confirm connector points align loft If necessary, reposition the connector points of profiles to align loft. Fig. 48 Click OK in the Property Manager. Step 5. Save. Use Ctrl-S. Fig. 49 Fig. 50 SOLIDWORKS 15 Hanger SKATEBOARD Page 3-12

13 N. Sketch8 Axle Hole. Step 1. Hide Planes 3, 4 and 5. To hide, in the Feature Manager Display Pane under Hide/Show column for Planes 3-5 click Show to turn off show, Fig. 51. Step 2. Change transparency of Loft1. To change transparency, move cursor to activate Loft1 row in the Feature Manager Display Pane and under Transparency column click Transparency to toggle transparency, Fig. 51. Step 3. Click Right Plane in the Feature Manager and click Sketch on the Context toolbar, Fig. 51. Step 4. Click Normal To on the Standard Views toolbar. (Ctrl-8) Fig. 51 Origin Step 5. Click Circle on the Sketch toolbar. Step 6. Draw a circle starting at the Origin, Fig. 52. Step 7. Click Smart Dimension Step 8. Dimension circle diameter 8, Fig. 52. (S) on the Sketch toolbar. Fig. 52 Step 9. Click Isometric on the Standard Views toolbar. (Ctrl-7) Step 10. Click Extruded Cut on the Features toolbar. Step 11. In the Cut-Extrude Property Manager set: under Direction 1, Fig. 53 End Condition Through All - Both click OK. Fig. 53 Step 12. Save. Use Ctrl-S. Fig. 54 SOLIDWORKS 15 Hanger SKATEBOARD Page 3-13

14 O. Create Axis. Step 1. Click Reference Geometry on the Features toolbar and Axis from the menu. Step 2. In the Axis Property Manager set: under Selections, Fig. 55 click inside cylindrical face of axis hole, Fig. 56 click OK Cancel. and P. Create Plane6 for Pivot Pin. Step 1. Click Right on the Standard Views toolbar. (Ctrl-4) Step 2. Ctrl click Top Plane and Axis1 in the Feature Manager to select both, Fig. 57. Fig. 56 Fig. 55 Step 3. Click Reference Geometry on the Features toolbar and Plane from the menu. Step 4. In the Plane Property Manager set: under First Reference, Fig. 58 Top Plane is selected click At Angle Angle 20 under Second Reference Axis1 is selected click OK. Top Plane Fig. 57 New Plane6 Fig. 58 Fig. 59 SOLIDWORKS 15 Hanger SKATEBOARD Page 3-14

15 Q. Create Sketch9 Circle in Plane6 for Pivot Pin. Step 1. Hide Plane6. To hide, in the Feature Manager Display Pane under Hide/Show column for Plane6 click Show to turn off show, Fig. 60. Step 2. Click Plane6 in the Feature Manager and click Sketch on the Context toolbar, Fig. 60. Step 3. Click Normal To Step 4. Click Circle on the Views toolbar (Ctrl-8). (S) on the Sketch toolbar. Step 5. Draw a circle starting at the Origin, Fig. 61. Origin Fig. 60 Step 6. Click Smart Dimension (S) on the Sketch toolbar. Step 7. Dimension diameter 11.5, Fig. 61. Step 8. Click Right Step 9. Click Features on the Standard Views toolbar. Fig. 61 on the Command Manager toolbar. Step 10. Click Extruded Boss/Base on the Features toolbar. Step 11. In the Property Manager set: under From, Fig. 62 Start Condition Offset Offset Value 5 click Reverse Direction Fig. 62 under Direction 1 Depth 34 click Reverse Direction click Draft On and 2º (inward) click OK. Fig. 63 SOLIDWORKS 15 Hanger SKATEBOARD Page 3-15

16 R. Create Plane7 for Rib. Step 1. Ctrl click Plane6 and Axis1 in the Feature Manager to select both, Fig. 64. Select Plane6 first. Step 2. Click Reference Geometry on the Features toolbar and Plane from the menu. Step 3. In the Plane Property Manager set: under First Reference, Fig. 65 Top Plane is selected click Perpendicular under Second Reference click Axis1 is selected click OK. S. Sketch10 in Plane7 for Rib. Step 1. Hide Axis1. To hide, in the Feature Manager Display Pane under Hide/Show column for Axis1 click Show to turn off show, Fig. 67. Fig. 64 Fig. 66 Fig. 65 Plane6 New Plane7 Step 2. Hide Plane7. To hide, in the Feature Manager Display Pane under Hide/Show column for Plane7 click Show to turn off show, Fig. 67. Step 3. Click Plane7 in the Feature Manager and click Sketch on the Context toolbar, Fig. 67. Step 4. Click Normal To on the Views toolbar (Ctrl-8). Fig. 67 SOLIDWORKS 15 Hanger SKATEBOARD Page 3-16

17 Step 5. Click Style Spline in the Spline flyout on the Sketch toolbar. Step 6. Draw a 3 control vertex point Spline between underside silhouette edge of hanger and silhouette side edge pivot pin, Fig. 68. To draw spline, move cursor to bottom silhouette edge under hanger and when edge turns orange, click for 1st control vertex point. For 2nd spline point move cursor to left and down and click. Move cursor to left silhouette edge of pivot pin, when edge turns orange, click for 3rd control vertex point. Press Escape to end spline. Step 7. Click Smart Dimension (S) on the Sketch toolbar. Step 8. Dimension control vertex points, Fig Fig. 68 Step 9. Rotate view to view underside loft and pivot pin, hold down middle mouse button (wheel) and drag to rotate view. Step 10. Click Features Step 11. Click Rib Fig. 69 on the Command Manager toolbar. on the Features toolbar. Step 12. In the Rib Property Manager set: under Parameters, Fig. 70 Both sides Rib thickness 3 check Flip material side Fig. 70 click Draft On 6º check Draft outward click OK. Fig. 71 SOLIDWORKS 15 Hanger SKATEBOARD Page 3-17

18 T. Mirror Rib. Step 1. Ctrl click Right Plane and Rib1 feature in the Feature Manager to select both, Fig. 72. Step 2. Click Mirror toolbar. on the Features Step 3. Click OK Mirror Property Manager, Fig. 73 and Fig. 75. U. Fillet Edges. Step 1. Click Fillet toolbar. on the Features Fig. 72 Fig. 73 Step 2. In the Fillet Property Manager set: select FilletXpert, Fig. 74 set Radius 1 click the bottom edges of ribs, Fig. 75 click Apply R 1 Fig. 74 Fig. 75 Step 3. Radius 2.2, Fig. 76 click other edges of ribs on both sides, Fig. 77. Click Apply. R 2.2 Fig. 77 SOLIDWORKS 15 Hanger SKATEBOARD Page 3-18 Fig. 76

19 Step 4. Continue and add Fillets: Top edge of pivot pin on both sides, Radius 5, Fig. 78. Step 5. Bottom edge of pivot pin, Radius 4.5, Fig. 79. R 5 Fig. 78 R 4.5 Fig. 79 Step 6. Both edges of the bottom kingpin counterbore, Radius.25, Fig. 80. R.25 Fig. 80 SOLIDWORKS 15 Hanger SKATEBOARD Page 3-19

20 Step 7. Click Isometric on the Standard Views toolbar. (Ctrl-7) Step 8. Bottom inside edge of lofted cut, Radius 1.7, Fig. 81. Step 9. Top edge of lofted cut, Radius 1.2, Fig. 82. R 1.7 R 1.2 Fig. 81 Fig. 82 Step 10. Both end edges of loft, Radius 2, Fig. 83. Click OK Step 11. Save. Use Ctrl-S. R 2 Fig. 83 Fig. 84 SOLIDWORKS 15 Hanger SKATEBOARD Page 3-20

21 V. Appearance. Step 1. Click Render Tools on the Command Manager toolbar. Step 2. Click Preview Window 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. 85. Step 5. Over in the Appearances Property Manager set: click Advanced button, Fig. 86 under Color click gray swatch above black. Fig. 87 Fig. 85 Fig. 86 SOLIDWORKS 15 Hanger SKATEBOARD Page 3-21

22 Step 6. Click the Mapping tab, Fig. 88 under Mapping Mapping Type Automatic under Size/Orientation Width 60 press ENTER key, Fig. 89 Fig. 89 Step 7. Click Surface Finish tab, Fig. 90 under PhotoView Surface Finish check Bump Mapping Bump Strength.1 click OK. Fig. 88 Step 8. Save. Use Ctrl-S. Fig. 90 Fig. 91 SOLIDWORKS 15 Hanger SKATEBOARD Page 3-22

23 W. Decal. Step 1. Click Preview Window on the Render Tools toolbar to close. Step 2. Click Back on the Standard Views toolbar. (Ctrl-2) Step 3. Use Alt-Arrow Right key until view rotated 180º, Fig. 94. Step 4. Click Edit Decal on the Render Tools toolbar. Step 5. In the Decals Property Manager Image tab: under Decal Preview, Fig. 92 click Browse and My Documents buttons open cudacountry-hanger.png (find bit-map on cudacountry web page) under Mask Image select Use decal image alpha channel Step 6. Click Mapping tab at top of Decals Manager under Selected Geometry, Fig. 93 unselect all but Select Faces click face of Loft, Fig. 94 under Mapping, Fig. 93 Mapping type Label Vertical location -7 under Size/Orientation Fig. 92 Width 117 Rotation 0 click OK. Fig. 93 Step 7. Save. Use Ctrl-S. Face Fig. 94 SOLIDWORKS 15 Hanger SKATEBOARD Page 3-23