Tutoriais SolidWorls
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  • 1. F1 Car Chapter 2 Body A. Save as "BODY". Step 1. If necessary, open your BLANK file. Step 2. Click File Menu > Save As. Step 3. Key-in BODY for the filename and press ENTER. B. Side Cut. Step 1. Click Wireframe on the View toolbar. Fig. 1 Step 2. Click Right (plane) in the Feature Manager and click Sketch from the Content toolbar, Fig. 1. Step 3. Click Normal To on the Standard Views toolbar. (Ctrl-8) Step 4. Click Line (L) on the Sketch toolbar. ) Step 5. Draw the 4 lines in Fig. 22. Keep the lines away from the cartridge hole. Use the inferencing line, the dotted line that appears when you draw the Fig. 2 lines. Step 6. Click Spline (S) Spline on the Sketch toolbar. Step 7. Draw a spline across Fig. 3 the top, Fig. 3. Press Escape to end the spline. Control Point Step 8. Click the spline to dis- play the Spline Points (green) and Control Polygon. Fig. 4 Step 9. Click a gray Control Point to activate it and the Control Point turns yellow. Move the yel- low Control Point to adjust spline, Fig. 4. 10/16/09 SolidWorks 08 Body F1 CAR Page 2-1 Brookside Middle School Tech Ed http://www.sarasota.k12.fl.us/brookside/cudacountry email:cudacountry@comcast.net
  • 2. Step 10. Click Smart Dimen- sion (S) on the Sketch toolbar. Step 11. Dimension as shown Fig. 5. To Smart di- Fig. 5 mension click the line to dimension, then move the cursor up off the sketch and click. Key- in the dimension and press ENTER. To Smart dimension the over all length, 195, click the back corner and click the front line. Move the cursor up off the sketch and click. Key-in 195 for the dimension and press ENTER. Step 12. Click Features on the Command Direction arrow Manager toolbar. Step 13. Click Extruded Cut on the Features Fig. 7 toolbar. Step 14. In the Extrude Property Manager: under Direction 1 End Condition to Through All The Direction arrow should point towards area to be cut away, Fig. 7. If arrow is pointing in wrong direction, click Flip side to cut, Fig. 6. Click OK Fig. 6 Fig. 8 Step 15. Save. Use Ctrl-S. C. Rear Cut. Back face Step 1. Click Back on the Standard Views toolbar. (Ctrl-2) Step 2. Click the back face of the body and click Sketch on the Content menu, Fig. 9. Step 3. Click Centerpoint Arc (S) in the Arc flyout on the Sketch toolbar. Fig. 9 SolidWorks 08 Body F1 CAR Page 2-2
  • 3. Step 4. Start arc at center of the cartridge hole and move 3. Drag around the cursor to the right. Click to place the first end and click to 2. Click point, then move cursor counterclockwise 180 de- end arc end point grees. Click to place the second end point, Fig. 10. Step 5. Click Line (L) on the Sketch toolbar. 1. Start at axle center Step 6. Draw the 4 lines in Fig. 11. Start the line at the end of the arc. Use the inferencing line, the dotted line Fig. 10 that appears when you draw the lines. Step 7. Click Smart Dimension (S) on the Sketch toolbar. Step 8. Dimension arc 13, Fig. 12. Step 9. Click Features on the Command Manager toolbar. Fig. 11 Step 10. Click Extruded Cut on the Features toolbar. Direction arrow Step 11. In the Extrude Property Manager: under Direction 1 End Condition to Through All The Direction arrow should point towards area to be cut away, Fig. 13. If arrow is pointing in Fig. 12 wrong direction, click Flip side to cut, Fig. 14. Click OK . Step 12. Click Isometric on the Stan- dard Views toolbar. Step 13. Save. Use Ctrl-S. Fig. 13 Fig. 14 SolidWorks 08 Body F1 CAR Page 2-3
  • 4. D. Top Cut. Top face Step 1. Click the top flat face of the body and click Sketch on the Content menu, Fig. 15. Step 2. Click Normal To on the Standard Views toolbar. (Ctrl-8) Step 3. Click Centerline in the Line flyout (S) on Fig. 15 the Sketch toolbar. Step 4. Starting from midpoint of the bottom of the sketch, draw a centerline up through the sketch, Fig. 16. Step 5. Press the Escape key to unselect Cen- terline. Step 6. Click the centerline to select it, Fig. 16. Centerline Step 7. Click Dynamic Mirror on the Sketch toolbar or Tools Menu > Sketch Tools > Dynamic Mirror, Fig. 16. Symmetry symbols appear at both ends of the centerline. Geometry drawn on one side of mirror centerline will mirror onto the other side. Dynamic Mirror Step 8. Click Line (L) on the Sketch Fig. 16 Fig. 17 toolbar. Step 9. Draw the 5 lines in Fig. 17. Keep the vertical line away from the blank. Avoid any infer- encing lines except vertical. SolidWorks 08 Body F1 CAR Page 2-4
  • 5. Step 10. Click Smart Dimension (S) on the Sketch toolbar. Step 11. Add dimensions as shown in Fig. 18. Start at the top, with the 40. Dimension the distance between the side pod edge and the edge of Blank 2. 1 2 Step 12. Click Tangent Arc in Fig. 19 the Arc flyout on the Sketch toolbar. Step 13. Draw an arc between the Posi- tion 1 and Position 2, Fig. 19. Step 14. Click Features on the Fig. 18 Command Manager toolbar. Step 15. Click Extruded Cut on the Features toolbar. Direction arrow Step 16. In the Extrude Property Manager: under Direction 1 End Condition to Through All The Direction arrow should point towards area to be cut away, Fig. 20. If arrow is pointing in wrong direction, click Flip side to cut, Fig. 21. Fig. 20 Fig. 21 Click OK . Step 17. Click Isometric on the Standard Views toolbar. Step 18. Click Shaded With Edges on the View toolbar. Step 19. Save. Use Ctrl-S. Fig. 22 SolidWorks 08 Body F1 CAR Page 2-5
  • 6. E. Under Front Wheel Cut. Step 1. Rename Features in the Feature Manager (left panel). To rename, click the Feature name and press F2, Fig. 23. Change: BODY CARTRIDGE HOLE AXLE HOLES EYE SCREW SLOT SIDE CUT REAR CUT TOP CUT Fig. 23 Step 2. Click Right (plane) in the Feature Manager and click Sketch from the Content toolbar, Fig. 23. Step 3. Click Normal To on the Standard Views toolbar. (Ctrl-8) Step 4. Click Spline (S) on the Sketch toolbar. Step 5. Draw a 3 point spline across the bottom in front of the axle, Fig. 24. Allow room for the front wing, above and between the spline and the nose tip. Also, allow for the wheel stand- offs around the axle hole. Press Escape to end the spline. Point 2 Point 1 Step 6. Click the spline to display the Spline Point 3 Points (green) and Control Polygon. Fig. 24 Step 7. Click a gray Control Point to activate it and the Control Point turns yellow. Move the yellow Control Point to adjust spline, Fig. 25. Fig. 25 Step 8. Click Features Direction on the Command Manager arrow toolbar. Step 9. Click Extruded Cut Fig. 26 on the Features toolbar. Step 10. In the Extrude Property Man- ager: under Direction 1 End Condition to Through All Fig. 27 Fig. 28 The Direction arrow should point towards area to be cut away, Fig. 26. If arrow is pointing in wrong direction, click Flip side to cut, Fig. 27. Click OK . SolidWorks 08 Body F1 CAR Page 2-6
  • 7. F. Loft Cockpit. Step 1. Rename Features in the Feature Manager. To rename, click the Feature name and press F2, Fig. 29. Change: Extrude 4 to FRONT WHEEL Top face CUT. Step 2. Click the top face of the body and click Sketch on the Content Fig. 29 menu, Fig. 30. Fig. 30 Step 3. Click Normal To on the Standard Views toolbar. (Ctrl-8) Step 4. Click Zoom to Selection (Q) on the View toolbar to zoom around the front of cockpit, Fig. 31. Step 5. Click Centerline in the Line flyout (S) on the Sketch toolbar. Zoom Step 6. Starting from midpoint of the cartridge arc Centerline edge, draw a centerline down through the sketch, Fig. 32. Dynamic Step 8. With the centerline selected, click Dynamic Mirror Mirror on the Sketch toolbar or Fig. 31 Fig. 32 Tools Menu > Sketch Tools > Dynamic Mirror, Fig. 32. Position 1 Position 2 Step 9. Click Line (L) on the Sketch toolbar. Step 10. Draw the 2 lines in Fig. 33. Start the first line at top endpoint of centerline, Position 1, Fig. 33. Bring the Position 3 line over to the corner, Position 2. Continue another line down vertically, Position 3. Step 11. Click Spline (S) on the Sketch toolbar. Fig. 33 SolidWorks 08 Body F1 CAR Page 2-7
  • 8. Step 12. Draw a spline from the end of the vertical line to the center- line, Fig. 34. Press Escape to end the spline. Step 13. Shift click a vertical line and a spline to select both, Fig. 34. Line To Shift click, click a vertical line, then hold down the Shift key and click the spline. Spline Step 14. Click Tangent on the Content menu, Fig. 35. Fig. 34 Step 15. Click a gray Control Point to activate it and the Control Point turns yellow. Move the yellow Control Point to adjust spline, Fig. 35. Step 16. Click Smart Dimension (S) on the Sketch toolbar. Step 17. Dimension as shown Fig. 36. Step 18. Click Exit Sketch on the Sketch toolbar. Fig. 35 Step 19. Click Isometric on the Standard Views toolbar. Step 20. Click the top face of the body, Fig. 37. Step 21. Click Insert Menu > Reference Geometry > Plane. Step 22. In the Plane Property Manager, under Selections: Set Offset Distance to 7 click OK in the Property Manager, Fig. 38. Fig. 36 Top face Fig. 37 Fig. 38 SolidWorks 08 Body F1 CAR Page 2-8
  • 9. Step 23. Click the cockpit sketch (Sketch 9) in the Feature Manager, Fig. 39 and copy. Use Ctrl-C to copy sketch. Step 24. Click the new Plane (Plane1) in the Feature Man- ager, Fig. 40 and paste sketch. Use Ctrl-V to paste sketch, Fig. 41. Step 25. Click the Sketch10 (pasted sketch) in the Feature Manager and click Edit Sketch on the Con- tent menu, Fig. 41. Fig. 39 Fig. 40 Step 26. Click Normal To on the Standard Views toolbar. (Ctrl-8) Step 27. Click Zoom to Selection (Q) on the View toolbar to zoom Sketch around cockpit. Step 28. Click the top left corner of the sketch and click Make Fixed on the Content menu, Fig. 42. Fig. 41 Fig. 42 Step 29. Change dimension of line Click corner from 23 to 14, Fig. 43. to fix Step 30. Click Exit Sketch on the Sketch toolbar. Fig. 43 Fig. 44 SolidWorks 08 Body F1 CAR Page 2-9
  • 10. Step 31. Click Isometric on the Standard Views toolbar. Step 32. Click Loft Base/Boss on the Features toolbar. Step 33. Click both sketches, Fig. 45. Step 34. In the Loft Property Manager, Sketch under Options check Merge results, Fig. 46 and click OK Sketch . G. Create Folder for Loft. Fig. 45 Step 1. Click the Plane1 in the Feature Fig. 46 Manager and click Hide on the Content menu, Fig. 47. Step 2. Shift click Plane1 and Loft1 in the Feature Manager to select both. Right click and click Add to New Folder on the menu, Fig. 48. Step 3. Rename new Folder LOFT COCKPIT in the Feature Manager. To rename, click the Fig. 49 Folder name and press F2, Fig. 49. Fig. 47 Fig. 48 H. Loft Cartridge Front. Step 1. Click the front face of the cartridge hole arc and click Sketch on the Content menu, Fig. 50. Step 2. With the front face still selected, click Convert Entities on the Sketch toolbar. Front face Step 3. Click Exit Sketch on the Sketch toolbar. Fig. 50 SolidWorks 08 Body F1 CAR Page 2-10
  • 11. Step 4. Click the top face of cockpit loft and click Sketch on the Content menu, Fig. 51. Top face Step 5. Click Normal To on the Standard Views toolbar. (Ctrl-8) Step 6. Click Zoom to Selection (Q) on the View toolbar to zoom around the front of cockpit, Fig. 52. cockpit Fig. 51 Step 7. Click Centerline in the Line flyout (S) on the Sketch toolbar. Dynamic Mirror Step 8. Starting from midpoint of the car- Centerline tridge arc edge, draw a centerline down through the sketch, Fig. 53. Zoom Step 9. With the centerline selected, click Dynamic Mirror on the Fig. 53 Position 1 Sketch toolbar or Tools Menu > Position 2 Sketch Tools > Dynamic Mirror, Fig. 53. Symmetry symbols appear Position 3 Fig. 52 at both ends of the centerline. Geometry drawn on one side of mirror centerline will mirror onto the other side. Step 10. Click Line (L) on the Sketch toolbar. Step 11. Start first line top endpoint of centerline , Position 1, Fig. 54. Bring the line over to the corner, Position 2. Fig. 54 Continue another line down vertically, Position 3. The lines will mirror over to the other side of the Dynamic Mirror centerline. Start arc Step 12. Click Centerpoint Arc (S) in the Arc flyout on the Sketch toolbar. Step 13. Start arc on centerline aligned with the end of verti- cal line and move the cursor to the left. Click to place the first end point, then move cursor counterclockwise Fig. 55 90 degrees. Click to place the second end point, Fig. 55. SolidWorks 08 Body F1 CAR Page 2-11
  • 12. Step 14. Click Smart Dimension (S) on the Sketch toolbar. Step 15. Dimension line 11 and arc radius 13 as shown in Fig. 56. Step 16. Click Exit Sketch on the Sketch toolbar. Step 17. Click Isometric on the Standard Views toolbar. Fig. 56 Step 18. Click Loft Base/Boss on the Features toolbar. Step 19. Click the offset entities sketch and the sketch on top face, Fig. 57. Step 20. In the Loft Property Manager, under Start/End Constraints: Set Start constraint: Tangency to Face Sketch 1 Set Start Tangent Length: .9 Fig. 57 and Fig. 58 Sketch 2 click OK in the Prop- erty Manager. Fig. 57 Step 21. Save. Use Ctrl-S. I. Create Side Pod Construction Sketch. Step 1. Click the side face of body (side pod), Fig. 59. Step 2. Click Insert Menu > Surface > Offset. Fig. 58 Step 3. In the Property Manager, set: Offset distance to 3, Fig. 60 and click OK . Side face Fig. 59 Fig. 60 SolidWorks 08 Body F1 CAR Page 2-12
  • 13. Step 4. Click the new surface and click Sketch on the Content menu, Fig. 61. Step 5. Click Offset Entities on the Sketch toolbar. Step 6. In the Offset Entities Property Manager set: Distance to 3 Surface The yellow offset rectangle should be on the out- Fig. 61 side of the face, Fig. 62. If it is not, click Reverse. Click OK . Step 7. Click Surface-Offset1 in the Feature Manager and click Hide on the Content menu, Fig. 63 and Fig. 64. Step 8. Click Exit Sketch on the Sketch toolbar. J. Create Side Pod 3D Sketch. Step 1. Use the Rotate View in the View toolbar to rotate view as shown in Fig. 64. Fig. 62 Fig. 63 Step 2. Use the Zoom to Area in the View toolbar to drag a zoom window around the left side pod, Fig. 64. Step 3. Click 3D Sketch in the Sketch Zoom flyout on the Sketch toolbar. Be sure to click Fig. 64 the flyout arrow to select 3D Sketch. Step 4. Click Spline (S) on the Sketch toolbar. ) 1 The cursor should change to XY plane indicating you are sketching in XY plane. If not, press Tab to switch sketch plane. Step 5. Click to start spline at the top corner (vertex) of body and side pod, Position 1, Fig. 65. Fig. 65 2 Step 6. Click 2nd endpoint of spline on the back vertical line of the 2D sketch, Position 2. Keep the endpoint away from the midpoint of the line. Press Escape to end Spline, Fig. 65. SolidWorks 08 Body F1 CAR Page 2-13
  • 14. Step 7. Press S key again and select Spline . Step 8. Press Tab to change the sketch plane to the 3 YZ plane . View the Reference Triad at the bottom left corner of the display Fig. 66 2 to determine the sketch plane. Step 9. Draw a spline from Position 2 on the back 4 vertical line of 2D sketch to front vertical line, Position 3, Fig. 66. Press Escape to end Spline. 3 Step 10. Press S key again and select Spline . Step 11. Use the right arrow to rotate view as shown in Fig. 67. Fig. 67 Step 12. Draw a spline from Position 3 on the front 4 vertical line of 2D sketch to top corner (ver- tex) of body and side pod, Position 4, Fig. 67. Press Escape to end Spline. 1 Step 13. Click Line (L) on the Sketch toolbar. Step 14. Draw a line across the top of the body to con- nect the ends of the splines, Position 1 to Fig. 68 Position 4, Fig. 68. Press the Escape key to unselect Line. Step 15. Click Smart Dimension (S) on the Sketch toolbar. Step 16. Add dimensions between endpoints of spline and top corner of the 2D sketch as shown in Fig. 69. To Smart dimension, the end of spline point and the top corner of 2D Fig. 69 sketch. SolidWorks 08 Body F1 CAR Page 2-14
  • 15. Step 17. Press the Escape key to unselect Smart Dimension. Step 18. Click Back on the Standard Views toolbar. (Ctrl-2) Step 19. Click the lower spline to display the Spline Points (green) and Control Polygon. Step 20. Click a gray Control Point to activate it and the Control Fig. 70 Point turns yellow. Move the yellow Control Point to adjust spline, Fig. 70. Step 21. Click Right on the Standard Views toolbar. (Ctrl-4) Step 22. Use the Control Points to adjust spline, Fig. 71. Step 23. Click Front on the Standard Views Fig. 71 toolbar. (Ctrl-1) Step 24. Use the Control Points to adjust top spline, Fig. 72. Step 25. Be careful when adjusting the splines. The splines must be keep out away from the body or the surface created from this 3D sketch will not cut the body. Avoid this er- ror by adjusting spline in each view (Normals). Check splines in top view. Fig. 73 is correct, but Fig. 74 has Fig. 72 error. Keep splines outside body Step 26. Click Isometric on the Standard Views toolbar. Step 27. Exit the 3D Sketch. To Exit, click in the Sketch flyout on the Sketch toolbar. Click the flyout arrow then 3D Sketch. Fig. 73 Fig. 74 SolidWorks 08 Body F1 CAR Page 2-15
  • 16. K. Create Fill Surface. Step 1. Click Insert Menu > Surface > Fill. Step 2. Select the 3D Sketch, Fig. 75. Click OK in the Property Manager, Fig. 76. 3D Sketch L. Cut with Surface. Fig. 75 Step 1. Click Insert Menu > Cut > With Surface. Step 2. In the SurfaceCut Property Manager: click cut surface in drawing, Fig. 77 77. Fig. 76 the Direction arrow should point towards area to be cut way, Fig. 77 if arrow is pointing in wrong direction, click Flip Cut , Fig. 78 Direction arrow click OK . Surface Fig. 77 Fig. 78 Step 3. Click Surface-Fill1 in Feature Manager and click Hide on the Content menu, Fig. 79. Step 4. Expand Surface-Fill1 in Feature Manager, click 3DSketch1 and click Hide on the Content menu, Fig. 80. M. Copy Side Pod 3D Sketch. Step 1. Click 3DSketch1 in the Feature Manager, Fig. 81. Step 2. With the 3D Sketch selected, use Ctrl-C to copy 3D Sketch. Step 3. Use Ctrl-V to paste 3D Sketch. Fig. 79 Fig. 80 Step 4. Click the new copied 3D Sketch in the Feature Manager and click Edit Sketch on the Content menu, Fig. 82. Fig. 81 Fig. 82 SolidWorks 08 Body F1 CAR Page 2-16
  • 17. Step 5. Click Isometric on the Standard Views toolbar. Zoom Step 6. Rotate View and Zoom to Area Fig. 83 around side pod, Fig. 83. Step 7. Pull down the vertex at the top corners of line and spline, Positions 1 and 4 down to the bottom of body, Fig. 84. Keep the vertex in the corner (edge). If the vertex is not at the bottom the surface will not cut. 4 Pull vertex of spline down Step 8. Click Smart Dimension (S) on to bottom Fig. 84 1 the Sketch toolbar. Step 9. Change the front dimension to 20 and the back dimension to 23 at the corners be- tween endpoints of spline and top corner of the 2D sketch as shown in Fig. 85. Step 10. Press the Escape key to unselect Smart Dimension. Fig. 85 Step 11. Click Back on the Standard Views toolbar. (Ctrl-2) Keep splines Step 12. Click the bottom spline to dis- outside body play the Spline Points (green) and Control Polygon. Step 13. Click a gray Control Point to activate it and the Control Point turns yellow. Move the Fig. 86 yellow Control Point to adjust spline, Fig. 86. Step 14. Click Front on the Stan- dard Views toolbar. (Ctrl-1) Step 15. Use the Control Points to ad- just spline, Fig. 87. Fig. 87 Fig. 88 Step 16. Check the splines in the Top View , Fig. 88. The splines most be outside the body or the surface created from this 3D sketch will not cut the body. SolidWorks 08 Body F1 CAR Page 2-17
  • 18. Step 17. Click Isometric on the Standard Views toolbar. Step 18. Exit the 3D Sketch. To Exit, click in the Sketch flyout on the Sketch toolbar. Click the flyout arrow then 3D Sketch. N. Create Lower Fill Surface. Step 1. Click Insert Menu > Surface > Fill. Step 2. Select the 3D Sketch, Fig. 89. Click OK in the Property Manager, Fig. 90. O. Cut with Lower Surface. 3D Sketch Step 1. Click Insert Menu > Cut > With Surface. Fig. 89 Step 2. In the SurfaceCut Property Manager: click cut surface in drawing, Fig. 91 91. the Direction arrow should point Fig. 90 towards area to be cut away, Fig. 91 if arrow is pointing in wrong direction, click Direction Flip Cut , Fig. 92 arrow Surface Fig. 92 click OK . Fig. 91 Step 4. Click Surface-Fill2 in Feature Manager and click Hide on the Content menu, Fig. 93. Step 5. Click Sketch13 (2D rectangle sketch) in the Feature Manager and click Hide on the Content menu, Fig. 94. Fig. 93 Fig. 94 SolidWorks 08 Body F1 CAR Page 2-18
  • 19. P. Mirror Side Pod. Step 1. Click Mirror on the Features toolbar. Step 2. In the Property Manager set: under Mirror Face/Plane, Fig. 96 expand the Design Tree in the top left corner of the drawing area click Right (Plane), Fig. 97 under Features to Mirror in Design Tree select SurfaceCut1 and SurfaceCut2 click OK , Fig. 98. Step 3. Save. Use Ctrl-S. Fig. 96 Fig. 97 Step 4. In the Feature Manager create folder for Side Pods. Fig. 98 To create folder select all features. Click the first feature, hold down Shift key and click last feature, Fig. 99. Step 5. Right click any selected feature and click Add to New Folder on the Con- tent menu (click OK to warning) Fig. 100. Step 6. Rename the folder SIDE Fig. 99 Fig. 100 Fig. 101 POD. To rename, select folder and use F2 key, Fig. 101. Q. Wheel Standoff. Step 1. Click Right (plane) in the Feature Manager and click Sketch from the Content toolbar, Fig. 102. Step 2. Click Normal To on the Standard Views toolbar. (Ctrl-8) Fig. 102 Step 3. Use the Zoom to Area in the View toolbar to drag a zoom window around the front axle hole, Fig. 103. Zoom Fig. 103 SolidWorks 08 Body F1 CAR Page 2-19
  • 20. Step 4. Click the edge of the front axle hole, Fig. 104. Convert edge to entities Step 5. Click Convert Entities on the Sketch toolbar. Step 6. Click Centerline in the Line flyout (S) on the Sketch toolbar. Fig. 104 Step 7. Draw two centerlines from the center of the circle as shown in, Fig. 105. Keep one centerline horizon- tal. Horizontal center- Step 8. Click Smart Dimension (S) on the Sketch toolbar. Fig. 105 Step 9. Dimension angle between construction lines 10 as shown in Fig. 106. To Smart dimension click both construction lines, then move the cursor and click. Key-in 10 for the dimension and press ENTER. Step 10. Click Ellipse on the Sketch toolbar. Horizontal center- Step 11. Draw an ellipse as shown in Fig. 107. To draw el- lipse, click the center of circle to place the center of Fig. 106 the ellipse. Drag to the angled center line and click to set the major axis. Drag down below circle and click again to set the minor axis. Major axis Step 12. Click Smart Dimension (S) on the Sketch toolbar. Minor axis Step 13. Dimension ellipse as shown in Fig. 108. To Smart dimension click the major axis points, then move Fig. 107 the cursor up off the sketch and click. Key-in 17 for the dimension and press ENTER. Dimension the minor diameter 8. Step 14. Save. Use Ctrl-S. Fig. 108 SolidWorks 08 Body F1 CAR Page 2-20
  • 21. Step 15. Zoom out, use the Z key and use Zoom to Area to drag a zoom window around the both axle holes, Fig. 109. Zoom Step 16. Press Escape to unselect Zoom. Fig. 109 Step 17. Copy sketch to rear axle. To Drag selection around sketch copy, drag selection around sketch, Fig. 110. Be sure to get the dimensions in selection. Hold down Ctrl key and drag from center of axle hole (circle) Ctrl Drag Ctrl Drag to to center of rear axle hole. from center Fig. 110 center of axle hole Step 18. Click Features n the Command Manager toolbar. Step 19. Use the Rotate View in the View toolbar to rotate view as shown in Fig. 111. Step 20. Click Extruded Boss/Base on the Features toolbar. Step 21. In the Property Manager set: under From Start Condition to Offset Offset Value to 3 under Direction 1 Depth to 16 click OK , Fig. 111 and Fig. 111 Fig. 112 Fig. 112. Step 22. Rename the Extruded Feature WHEEL STANDOFF. To rename, se- lect folder and use F2 key, Fig. 113. Fig. 113 SolidWorks 08 Body F1 CAR Page 2-21
  • 22. R Mirror Wheel Standoff. Step 1. Click Mirror on the Features toolbar. Step 2. In the Property Manager set: under Mirror Face/Plane, Fig. 114 expand the Design Tree in the top left corner of the drawing area click Right (Plane), Fig. 115 under Features to Mirror in Design Tree select WHEEL STANDOFF Fig. 114 click OK , Fig. 116. Fig. 115 Step 3. Save. Use Ctrl-S. Fig. 116 S. Fillet Top Edges. Step 1. Click Isometric on the Standard Views toolbar. (Ctrl-7) Step 2. Click Fillet on the Fea- tures toolbar. Edge Step 3. In the Fillet Property Manager: Edge Select FilletXpert, Fig. 117. 117 Fig. 118 Set the Radius to 3 Fig. 117 Click the inside edge on all 4 wheel standoffs on both sides of the body (hold down middle Edge mouse button to rotate view), Fig. 118. Edge Click Apply Fig. 120 Set the Radius to 1 Click the end edge on all 4 wheel standoffs, Fig. 120. Fig. 119 click OK , Fig. 121. Fig. 121 SolidWorks 08 Body F1 CAR Page 2-22
  • 23. T. Bottom Rear 3D Sketch. Snap to Centerline vertex Step 1. Click Back on the Standard Views toolbar. (Ctrl-2) Step 2. Click 3D Sketch in the Sketch flyout on the Sketch toolbar. Centerline Fig. 122 Start at Step 3. Click Centerline in the Line flyout (S) midpoint Draw arc on the Sketch toolbar. beyond center of body Step 4. Draw two centerlines as shown in Fig. 122. Snap endpoint to the vertex. Step 5. Click Centerpoint Arc (S) in the Arc flyout Fig. 123 on the Sketch toolbar. Step 6. Click the midpoint of top centerline (center of the cartridge hole) to start the arc and move the cursor to the left end of centerline. Click to place the first endpoint, then move cursor counterclockwise past 90 degrees or beyond middle of body. Click to place the second endpoint, Fig. 123. Draw line past centerline Fig. 124 Step 7. Click Line (L) on the Sketch toolbar. Step 8. Draw the line as shown in Fig. 124. Start line at mid- point of top centerline and continue line down past bottom centerline (origin). Trim 3 Step 9. Click Trim Entities on the Sketch toolbar. Fig. 125 Step 10. Trim the entities as shown in Fig. 126. To trim, click the entities you want to remove, Fig. 125. Fig. 126 SolidWorks 08 Body F1 CAR Page 2-23
  • 24. Step 11. Press Escape to unselect Trim Entities. Step 12. Use right arrow two times to rotate view as shown in 1 Fig. 127. Step 13. Click 3 Point Arc on the Sketch toolbar. 3 Step 14. Press Tab to change the sketch plane to the YZ plane 2 . Fig. 127 Step 15. Draw an arc between the Position 1, Position 2 and Posi- tion 3 shown in Fig. 127. To draw the arc, first click Posi- tion 1, then Position 2. Swing the arc to Position 3 and click. At Position 1 keep the arc inside the edge of the body. Step 16. Click Smart Dimension (S) on the Sketch toolbar. Fig. 128 Step 17. Dimension the endpoint of arc to the side pod 11 as shown Fig. 128 128. Step 18. Use up arrow two to rotate view as shown in Fig. 129. Step 19. Click 3 Point Arc on the Sketch toolbar. Step 20. Change the sketch plane to ZX . Use the tab key. 3 The cursor will change to ZX. 1 2 Step 21. Draw an arc between the Position 1, Position 2 and Posi- tion 3 to close the 3D Sketch as shown in Fig. 129. To Keep arc Fig. 129 inside edge draw the arc, first click of body Position 1, then Position 2. Swing the arc to Posi- tion 3 and click. At Posi- tion 1 keep the arc inside the edge of the body, Fig. 130 and Fig.131. Step 22. Exit the 3D Sketch. To Exit, click in the Sketch flyout Fig. 130 Keep arc Fig. 131 on the Sketch toolbar. Good inside edge Wrong of body SolidWorks 08 Body F1 CAR Page 2-24
  • 25. U. Create Bottom Rear Fill Surface. Step 1. Click Insert Menu > Surface > Fill. 3D Sketch Step 2. Select the 3D Sketch, Fig. 132. Click OK in the Property Manager, Fig. 133. V. Cut Bottom Rear Surface. Step 1. Click Insert Menu > Cut > With Sur- face. Fig. 132 Step 2. In the SurfaceCut Property Manager: click cut surface in drawing, Fig. 133 Fig. 134 Direction the Direction arrow should point arrow towards area to be cut away, Fig. 134 if arrow is pointing in wrong Surface direction, click Flip Cut , Fig. 135 click OK . Fig. 134 Fig. 135 Step 3. Click Surface-Fill3 in Feature Manager and click Hide on the Content menu, Fig. 136. The 3DSketch3 should hide itself. Fig. 136 SolidWorks 08 Body F1 CAR Page 2-25
  • 26. W. Mirror Bottom Rear. Step 1. Click Mirror on the Features toolbar. Step 2. In the Property Manager set: under Features to Mirror, Fig. 137 expand the Design Tree in the top left corner of the drawing area click Right (Plane), Fig. 138 under Features to Mirror in Design Tree select SurfaceCut3 Fig. 137 click OK , Fig. 138. Step 3. In the Feature Manager create a folder for BOTTOM REAR CUT. To cre- ate folder, first select all features, click Fig. 138 the first feature, hold down Shift key and click last feature, Surface-Fill3 to Mirror3, Fig. 140. Step 4. Right click any selected feature and Fig. 139 click Add to New Folder on the Con- tent menu (click OK to warning) Fig. 141. Step 5. Rename the folder BOT- TOM REAR CUT. To rename, select folder and use F2 key, Fig. 142. Fig. 140 Fig. 141 Fig. 142 SolidWorks 08 Body F1 CAR Page 2-26
  • 27. X. Front Wing. Step 1. Click Right (plane) in the Feature Manager and click Sketch from the Content toolbar, Fig. 143. Step 2. Click Normal To on the Standard Views toolbar. (Ctrl-8) Step 3. Use the Zoom to Area in the Fig. 143 View toolbar to drag a zoom window around the area in front of front axle, Fig. 144. Zoom Step 4. Click Line (L) on the Sketch Fig. 144 toolbar. Step 5. Draw the 2 lines in Fig. 145. Keep one line hori- zontal. Step 6. Click Smart Dimension (S) on the Sketch toolbar. Fig. 145 Step 7. Add the Dimensions as shown in Fig. 146. To Smart dimension the angle click the middle of the construction lines, then move the cursor and click. Key-in 18 for the dimension and press ENTER. Step 8. Click Offset Entities Fig. 146 on the Sketch toolbar. Offset Step 9. In the Offset Entities Property Manager set: Distance to 4 check Bi-directional click the angled line, Fig. 148 Fig. 147 Fig. 148 click OK . Step 10. Click Tools Menu > Sketch Tools > Construction Geometry. Step 11. Click all the lines to change lines to construction lines, Fig. 149. Fig. 149 SolidWorks 08 Body F1 CAR Page 2-27
  • 28. Step 12. Click Line (L) on the Sketch toolbar. Step 13. Draw line for front of wing as shown in Fig. 150. Step 14. Click 3 Point Arc (S) in the Arc flyout Fig. 150 on the Sketch toolbar. 2 3 1 Step 15. Draw 3 Point Arc between Points 1, 2 and 3, Fig. 151. Step 16. Draw 3 Point Arc between Points 2, 4 and 5, Fig. 152. Keep Point 4 away from the horizon- tal center line. Snap Point 5 to the construction Fig. 151 line at Point 5. Important Point 5 snaps to 2 centerline so it become tangent to the center- line. Step 17. Click Smart Dimension (S) on the 4 5 Sketch toolbar. Fig. 152 Step 18. Dimension the top arc 64, Fig. 153. Dimension the gap between the horizontal center line and the bottom arc 1 as shown in Fig. 153. Step 19. Click Sketch Fillet on the Sketch toolbar. Fig. 153 Step 20. In the Sketch Fillet Property Manager set: Radius to 1 , Fig. 154 click the corner shown in Fig. 155 Radius to 2 , Fig. 156 click the two corners shown in Fig. 157. To Fig. 154 Fig. 155 Sketch Fillet the bottom fillet, click the line and the bottom arc. Click OK to message deleting geometry relations. Fig. 156 Fig. 157 SolidWorks 08 Body F1 CAR Page 2-28
  • 29. Step 21. Click Features on the Command Manager toolbar. Step 22. Click Isometric on the Standard Views toolbar. Step 23. Click Extruded Boss/Base on the Features toolbar. Step 24. In the Property Manager set: under From Start Condition to Offset Offset Value to 3 under Direction 1 Depth to 28 click OK , Fig. 158 Step 25. Save. Use Ctrl-S. Fig. 158 Fig. 159 Y. Create Front Wing Endplate. Step 1. Rename Extrude1 to FRONT WING EXTRUDE in the Feature Manager. To rename, click the feature name and press F2, Fig. 160. Step 2. Click the side face of wing and click Sketch on the Content menu, Fig. 161. Fig. 160 Fig. 161 Side face Step 3. Click Offset Entities on the Sketch toolbar. Step 4. In the Offset Entities Property Manager set: Distance to 1, Fig. 162. The yellow offset sketch should be on the outside of the face, Fig. 163. If 163 it is not, click Reverse. Click OK . Fig. 162 Fig. 163 SolidWorks 08 Body F1 CAR Page 2-29
  • 30. Step 5. Click Features on the Command Manager toolbar. Step 6. Click Extruded Boss/Base on the Features toolbar. Step 7. In the Extrude Property Manager: Fig. 165 under Direction 1 Depth to 2.5 Reverse Direction The Direction arrow should Fig. 164 Fig. 166 point back towards the body, Fig. 165. If arrow is pointing in wrong direction, click Reverse Direction , Fig. 164. Click OK , Fig. 166. Z. Mirror Front Wing and Endplate. Step 1. Click Mirror on the Features toolbar. Step 2. In the Property Manager set: under Mirror Face/Plane, Fig. 167 expand the Design Tree in the top left corner of the drawing area click Right (Plane), Fig. 168 under Features to Mirror in Design Tree select FRONT WING EXTRUDE and Extrude 1 Fig. 167 Fig. 168 click OK , Fig. 169. Fig. 169 SolidWorks 08 Body F1 CAR Page 2-30
  • 31. AA. Create Front Wing Folder. Step 1. Ctrl click FRONT WING EXTRUDE, Extrude1 and Mirror4 in the Feature Manager to select all three. Right click any of the selected Features and click Add to New Folder on the menu, Fig. 170. Step 2. Rename new Folder WING FRONT in the Feature Manager. To rename, click the Folder name and press F2, Fig. 171. BB. Modify Rear Wing Sketch. Step 1. If necessary, turn on Instant3D on Fig. 170 Fig. 171 the Features toolbar. Step 2. Expand the WING FRONT folder. Hold down Ctrl key and drag FRONT WING EXTRUDE in the Feature Manager design tree out and set on the flat side face of the body just above the rear axle standout, Fig. 172. Step 3. Click Delete in Copy Confirmation dialog box to delete the external constraints (dimensions), Fig. 173. Step 4. Expand Extrude2 (rear wing), click Sketch17 in the Feature Manager and click Edit Sketch Plane from the Content toolbar, Fig. 174. Fig. 172 Fig. 173 Step 5. In the Sketch Plane Property Manager: Under Sketch Plane/Face, Fig. 175 Expand the Design Tree in the top left corner of the drawing area and click Right (Plane), Fig. 176. 176 Fig. 175 Click OK . Fig. 174 Fig. 176 SolidWorks 08 Body F1 CAR Page 2-31
  • 32. Step 6. Click Extrude2 (rear wing) in the Feature Manager and click Edit Sketch on the Content menu, Fig. 177. Step 7. Click Normal To on the Standard Views toolbar. (Ctrl-8) Step 8. Click Zoom to Selection (Q) on the View toolbar to zoom around the read wing sketch. sketch Step 9. Click Smart Dimension (S) on the Sketch toolbar. Fig. 177 Step 10. Add and change Dimensions as shown Fig. 178: Intersection of centerlines Add 31 dimension from bottom of body to inter- section of centerlines Add 23 dimension from rear of body to intersec- tion of centerlines Change length of angled centerline from 20 to 24 (length of sketch) Change angle of centerline from 18 to 14 Step 11. Click Exit Sketch on the Sketch toolbar. Fig. 178 CC. Modify Rear Wing Extrude. Step 1. Use the Rotate View in the View toolbar to rotate view as shown in Fig. 179. Step 2. Click the Extrude2 (rear wing) in the Feature Manag- rear er and click Edit Feature on the Content menu, Fig. 178. Fig. 179 Fig. 180 SolidWorks 08 Body F1 CAR Page 2-32
  • 33. Step 3. In the Property Manager set: Arc face under From set Start Condition to Surface/ Face/Plane set Select a Surface/Face/ Plane: click the outside arc face of the body at the cartridge hole, Fig. 182 Fig. 182 under Direction 1 End Condition to Offset From Surface set Face/Surface: expand the Design Tree in the top left corner of the drawing area click Right (Plane), Fig. 183 Fig. 183 Fig. 181 Depth to 31 click OK , Fig. 184. DD. Create Rear Wing Folder. Step 1. Rename Extrude2 to REAR WING EXTRUDE in the Feature Manager. To rename, click the Folder name and press F2, Fig. 185. Fig. 184 Step 2. Right click REAR WING EXTRUDE and click Add to New Folder on the menu, Fig. 186. Step 3. Rename new Folder WING REAR in the Feature Manager. To rename, click the Folder name and press F2, Fig. 187. Fig. 185 Fig. 186 Fig. 187 SolidWorks 08 Body F1 CAR Page 2-33
  • 34. EE. Create Rear Wing Endplate. Step 1. Click the side face of rear wing and click Sketch on the Content menu, Fig. 188. Step 2. Click Offset Entities on the Sketch toolbar. Side face Step 3. In the Offset Entities Property Manager set: Distance to 1 Fig. 188 The yellow offset sketch should be on the outside of the face, Fig. 190. If it is not, click Reverse. Click OK . Step 4. Click Features on Fig. 189 the Command Manager toolbar. Fig. 190 Step 5. Click Extruded Boss/Base on the Features toolbar. Step 6. In the Extrude Property Manager: under Direction 1 Depth to 2.5 Reverse Direction Fig. 191 Fig. 192 The Direction arrow should point back towards the body, Fig. 192. If arrow is pointing in wrong direc- tion, click Reverse Direction , Fig. 191. Click OK . Fig. 193 SolidWorks 08 Body F1 CAR Page 2-34
  • 35. FF. Mirror Rear Wing and Endplate. Step 1. Click Mirror on the Features toolbar. Step 2. In the Property Manager set: under Mirror Face/Plane, Fig. 194 expand the Design Tree in the top left corner of the drawing area click Right (Plane), Fig. 195 under Features to Mirror in Design Tree select REAR WING EXTRUDE and Extrude2 under Options check Geometry Pattern click OK , Fig. 196. Fig. 194 GG. Move Features to Rear Wing Folder. Step 1. In the Feature Manager, move the two features into the REAR WING Fig. 195 FOLDER. To move a feature, drag the feature over the last feature in the folder. When the cursor changes to Arrow release the feature, Fig. 197. Drag both Extrude2 and Mirror5 into the REAR WING FOLDER, Fig. 198. Fig. 196 HH. Fillet Edges. Step 1. Click Fillet on the Features toolbar. Fig. 197 Fig. 198 Step 2. In the Fillet Property Manager: Select FilletXpert, Fig. 199. FilletXpert 199 Set the Radius to 8 Click the edge between rear of side pod and body on both sides of the body (hold down middle mouse but- ton to rotate view), Fig. 200. Click Apply R8 Fig. 199 Fig. 200 SolidWorks 08 Body F1 CAR Page 2-35
  • 36. Set the Radius to 12, Fig. 201 Click the end edges on all 4 corners of side pods, Fig. 202. R 12 Continue and add Fillets: Fig. 202 R 12 Front edge of side pod and body, Radius 14, Fig. 203. Fig. 201 Top edge of body and side R 14 pod , Radius 1.5, Fig. 204. Fig. 203 Bottom edge of body and side pod, Radius 1.5, Fig. 205. Top back edge of cockpit, Radius 2, Fig. 206. Top front edge of cockpit, Radius 2, Fig. 207. R 1.5 R2 Fig. 204 Fig. 206 R 1.5 Fig. 205 R2 Fig. 207 SolidWorks 08 Body F1 CAR Page 2-36
  • 37. Bottom edge of cockpit (one side), Radius 2, Fig. 208. Bottom edge of cockpit (other side), Radius 2, Fig. 209. Both edges of endplate (all 4 endplates), Radius 1, Fig. 210. Edge of endplate and wing, Radius 1, Fig. 211. R2 Fig. 208 Edge of endplate and body, Radius 1, Fig. 212. 1 Click OK when done. R2 Fig. 209 R1 Fig. 210 R1 R1 R1 Fig. 211 Fig. 212 SolidWorks 08 Body F1 CAR Page 2-37