Delta Dart. Propeller. in the Feature Manager and click Sketch from the Content toolbar, Fig. 1. on the Sketch toolbar.

Transcription

1 Chapter 8 Delta Dart Propeller A. Base for Blade. Step 1. Click File Menu > New, click Part Metric and OK. Step 2. Click Top Plane in the Feature Manager and click Sketch from the Content toolbar, Fig. 1. Step 3. Click Center Rectangle (S) in the Rectangle flyout on the Sketch toolbar. Fig. 1 Step 4. Starting from the Origin draw a rectangle, Fig. 2. Step 5. Click Smart Dimension (S) on the Sketch toolbar. Step 6. Dimension rectangle 6.1 by 1.8, Fig. 3. Origin Step 7. Click Exit Sketch B. Save as "PROPELLER". Step 1. Click File Menu > Save As. on the Sketch toolbar. Step 2. Key-in PROPELLER for the filename and press ENTER. C. Create Plane. Step 1. Click Trimetric on the Standard Views toolbar. Step 2. Click Top Plane in the Feature Manager, Fig. 4. Step 3. Ctrl drag Top plane in graphics area up and release, Fig. 5. To Ctrl drag, hold down Ctrl and drag plane up. Fig. 2 Fig. 4 Fig. 3 Drag up Hold down Ctrl drag plane Fig. 5 2/27/13 SolidWorks 13 PROPELLER DELTA DART Page 8-1 Cudacountry.net Tech Ed cudacountry@hotmail.com

2 Step 4. In the Plane Property Manager set: Distance 67 and press ENTER, Fig. 6 click Zoom to Fit on the View toolbar the new plane should be above sketch, Fig. 7, if in wrong direction, check Flip, Fig. 6 click OK. Drag up set distance 67 D. Create Sketch in Plane 1. Step 1. Click Plane1 in the Feature Manager and click Sketch from the Content toolbar, Fig. 8. Step 2. Click Normal To toolbar. (Ctrl-8) Step 3. Click Center Rectangle on the Standard Views (S) on the Sketch toolbar. Fig. 6 Hold down Ctrl drag plane Fig. 7 Step 4. Starting from the Origin draw a rectangle, Fig. 9. Step 5. Click Smart Dimension Step 6. Dimension rectangle 16.5 by.65, Fig. 10. (S) on the Sketch toolbar. Fig. 8 Step 7. Click Exit Sketch Sketch toolbar. on the Plane1 E. Hide Plane1. Step 1. Click Trimetric on the Standard Views toolbar. Origin Step 2. Click Plane1 in graphic area on the Con- and click Hide tent menu, Fig. 11. Step 3. Save. Use Ctrl-S. Fig. 9 Fig. 10 SolidWorks 13 PROPELLER DELTA DART Page 8-2 Fig. 11

3 F. Guide Curve 1 Step 1. Click Right Plane in the Feature Manager and click Sketch from the Content toolbar, Fig. 12. Step 2. Click Normal To on the Standard Views toolbar. (Ctrl-8) Step 3. Click (S) on the Sketch toolbar. Fig. 12 Step 4. Draw a 2 Point from left endpoint of rectangle in Sketch 2 to left endpoint of rectangle in Sketch 1, Fig. 13. Press Escape to end spline. Step 5. Click spline to select it. Grab Circular handle (small gray dot) of Point 2 and pull handle out to left, Fig. 14 and Fig. 15. To find the Circular spline handle, start your cursor over the Point 2 and move up along the spline, just above the Origin the Circular spline will highlight as a red circle. Pull Circular Handle from here Point 2 Pull to here Step 6. Click Smart Dimension Fig. 13 Fig. 14 Fig. 15 (S) on the Sketch toolbar. Step 7. Dimension Point 2 Tangent Weighting1 80, Fig. 16. To dimension Tangent Weighting, click the Circular handle, then move the cursor out away from spline and click. Keyin 80 and press ENTER. Step 8. Dimension Point 2 Tangent Radial Direction 87 degrees, Fig. 17. To dimension Tangent Radial Direction, click the Circular handle and rectangle in Sketch 1, then move cursor left of sketch and click. Key-in 87 and press ENTER. Circular Handle Fig. 16 SolidWorks 13 PROPELLER DELTA DART Page 8-3 Fig. 17

4 Step 9. Click to display the Circular handle and locate the Circular handle of Point 1, Fig. 18. Step 10. Dimension Point 1 Tangent Weighting1 125, Fig. 19. To dimension Tangent Weighting, click the Circular handle, then move the cursor out away from spline and click. Key-in 125 and press ENTER. Fig. 18 Point 1 Circular Handle Fig. 19 Circular Handle Fig. 20 Step 11. Dimension Point 1 Tangent Radial Direction 95 degrees, Fig. 20. To dimension Tangent Radial Direction, click the Circular handle and rectangle in Sketch 2, then move cursor between and click. Key-in 95 and press ENTER. Step 12. Click Exit Sketch on the Sketch toolbar. G. Guide Curve 2 Step 1. Click Right Plane in the Feature Manager and click Sketch from the Content toolbar, Fig. 21. Step 2. Click (S) on the Sketch toolbar. Step 3. Draw a 2 Point from right endpoint of rectangle in Sketch 2 to right endpoint of rectangle in Sketch 1, Fig. 22. Press Escape to end spline. Fig. 21 SolidWorks 13 PROPELLER DELTA DART Page 8-4 Fig. 22

5 Step 4. Click spline to select it. Grab Circular handle (small gray dot) of Point 2 and pull handle out to right, Fig. 23 and Fig. 24. Step 5. Click Smart Dimension toolbar. (S) on the Sketch Pull Circular Handle from here Pull to here Circular Handle Step 6. Dimension Point 2 Tangent Weighting1 80, Fig. 25. To dimension Tangent Weighting, click the Circular handle, then move the cursor out away from spline and click. Key-in 80 and press ENTER. Step 7. Dimension Point 2 Tangent Radial Direction 87 degrees, Fig. 26. To dimension Tangent Radial Direction, click the Circular handle and rectangle in Sketch 1, then move cursor right of sketch and click. Key-in 87 and press ENTER. Fig. 23 Point 2 Fig. 24 Point 1 Fig. 25 Step 8. Dimension Point 1 Tangent Weighting1 125, Fig. 27. To dimension Tangent Weighting, click the Circular handle, then move the cursor out away from spline and click. Key-in 125 and press ENTER. Fig. 26 Fig. 27 Circular Handle Fig. 28 Step 9. Dimension Point 1 Tangent Radial Direction 95 degrees, Fig. 28. To dimension Tangent Radial Direction, click the Circular handle and rectangle in Sketch 2, then move cursor between and click. Key-in 95 and press ENTER. Step 10. Click Exit Sketch on the Sketch toolbar. SolidWorks 13 PROPELLER DELTA DART Page 8-5

6 H. Loft. Step 1. Click Trimetric Step 2. Click Features on the Standard Views toolbar. on the Command Manager toolbar. Step 3. Click Lofted Boss/Base on the Features toolbar. Step 4. In the Surface-Loft Property Manager set: under Profiles, Fig. 29 click the same position on the two rectangle sketches, Fig. 30 Sketch2 Sketch1 under Guide Curves click in the Guide Curves box click the two Guide Curve splines sketches, Fig. 30 and Fig. 31 Sketch3 Sketch4 click OK. Profile Sketch2 Fig. 29 Guide Curve Sketch3 Guide Curve Sketch4 Profile Sketch1 Fig. 30 Fig. 31 Fig. 32 SolidWorks 13 PROPELLER DELTA DART Page 8-6

7 I. Flex Blade. Step 1. Click Insert Menu > Features > Flex. Step 2. In the Flex Property Manager set: under Flex Input click the Loft in graphics area select Twisting, Fig. 33 Angle -73 degrees under Triad Y Rotation Origin -23 click OK. Step 3. Save. Use Ctrl-S. J. Hub. Step 1. Click Front Plane in the Feature Manager and click Sketch from the Content toolbar, Fig. 36. Fig. 33 Fig. 34 Fig. 35 Step 2. Click Normal To toolbar. (Ctrl-8) Step 3. Click Circle on the Standard Views (S) on the Sketch toolbar. Fig. 36 Step 4. Draw circle for the hub at Origin, Fig. 37. Step 5. Click Smart Dimension toolbar. (S) on the Sketch Step 6. Dimension circle diameter 4.15, Fig. 37. on the Command Man- Step 7. Click Features ager toolbar. Step 8. Click Extruded Boss/Base toolbar. on the Features Origin Fig. 37 SolidWorks 13 PROPELLER DELTA DART Page 8-7

8 Step 9. Click Trimetric on the Standard Views toolbar. Step 10. In the Property Manager set: under Direction 1, Fig. 38 End Condition Mid Plane Depth 10.7 check Merge result click OK, Fig. 39. K. Cut Hole. Step 1. Click the front face of the hub and click Sketch on the Content menu, Fig. 40. Fig. 38 Step 2. Click Circle (S) on the Sketch toolbar. Step 3. Draw a circle for the hole starting at the Origin, Fig. 41. Fig. 39 Step 4. Click Smart Dimen- Fig. 42 sion (S) on the Sketch toolbar. Step 5. Dimension circle diameter 1.2, Fig. 42. Step 6. Click Features Face on the Command Manager toolbar. Fig. 40 Fig. 41 Fig. 42 Step 7. Click Extruded Cut toolbar. on the Features Step 8. In the Cut-Extrude Property Manager set: End Condition Through All, Fig. 43 click OK. Step 9. Save. Use Ctrl-S. Fig. 43 SolidWorks 13 PROPELLER DELTA DART Page 8-8 Fig. 44

9 L. Fillet Blade Tip Edges. Step 1. Zoom in around blade tip, Fig. 45. To zoom, hold down Shift key and drag with middle mouse button (wheel). To pan, hold down Ctrl key and drag with middle mouse button (wheel). Zoom Step 2. Click Fillet on the Features toolbar. Step 3. In the Fillet Property Manager set: select FilletXpert, Fig. 46 Radius 2 click edges on top corners of blade, Fig. 47 click Apply, Fig. 46. M. Variable Fillet Blade Front. Step 1. Click Zoom to Fit (F) on the View toolbar. select Manual, Fig. 48 under Fillet type select Variable radius under Variable radius Parameters Radius.3 click left side edge, top edge and right side edge of blade, Fig. 49 click Set All button, Fig. 48. Fig. 46 Fig. 47 Top edge Fig. 45 Set the Unsigned Variable radius 1 at bottom, Fig. 49. The radius at top should be set to.3. To set radius, click Unsigned and key in radius and press ENTER. Click OK, Fig. 50. Click to set Left edge Click to set Right edge Fig. 48 Fig. 49 Fig. 50 SolidWorks 13 PROPELLER DELTA DART Page 8-9

10 N. Variable Fillet Blade Back. Step 1. Click Back on the Standard Views toolbar. (Ctrl-2) Step 2. Click Fillet on the Features toolbar. Step 3. In the Fillet Property Manager set: select Manual, Fig. 51 under Fillet type select Variable radius under Variable radius Parameters Radius.3 Top edge click left side edge, top edge and right side edge of blade, Fig. 52 click Set All button, Fig. 51. Set the Unsigned Variable radius 1 at bottom, Fig. 52. The radius at top should be set to.3. To set radius, click Unsigned and key in radius and press ENTER. Click OK, Fig. 53. Left edge Right edge Fig. 51 Fig. 52 Fig. 53 SolidWorks 13 PROPELLER DELTA DART Page 8-10

11 O. Fillet Hub. Step 1. Click Trimetric on the Standard Views toolbar. Step 2. Zoom in around hub, Fig. 54. To zoom, hold down Shift key and drag with middle mouse button (wheel). To pan, hold down Ctrl key and drag with middle mouse button (wheel). Step 3. Click Fillet on the Features toolbar. Step 4. In the Fillet Property Manager set: select FilletXpert, Fig. 55 Radius.3 click side edge of blade at hub, Fig. 56 click Right Loop Fig. 56 and Fig. 57 click Apply, Fig. 55 on the Fillet pop-up toolbar, Zoom Fig. 54 Fig. 55 Radius 1.6, Fig. 58 click rear cylindrical edge of hub, Fig. 59 click OK. Step 5. Save. Use Ctrl-S. Fig. 56 Fig. 57 Fig. 58 Fig. 59 Fig. 60 SolidWorks 13 PROPELLER DELTA DART Page 8-11

12 P. Circular Pattern for Blade. Step 1. Click Zoom to Fit (F) on the View toolbar. Step 2. Click View Menu > Temporary Axes. (Alt-V X) Step 3. Ctrl click the Loft1 and the first 4 Fillets in the Feature Manager, Fig. 61. To Ctrl click, click Loft1, then hold down the Ctrl key and click the first 4 Fillet features. Step 4. Click Circular Pattern Linear Pattern flyout on the Features toolbar. Be sure to click the flyout arrow to select Circular Pattern. in the Fig. 61 Step 5. In the Circular Pattern Property Manager set: under Parameters, Fig. 62 Fig. 62 Pattern Axis click Temp axis in graphics area, Fig. 63 and Fig. 64 Number of Instances 2 Fig. 63 Axis check Equal spacing under Options check Geometry pattern click OK. Axis Fig. 64 Fig. 65 SolidWorks 13 PROPELLER DELTA DART Page 8-12

13 Q. Sketch for Sweep Cut. Step 1. Turn off Temporary Axes. Click View Menu > Temporary Axes. (Alt-V X) Step 2. Click Trimetric Views toolbar. on the Standard Step 3. Zoom in around hub, Fig. 66. To zoom, hold down Shift key and drag with middle mouse button (wheel). To pan, hold down Ctrl key and drag with middle mouse button (wheel). Step 4. Click the front face of hub and click Sketch on the Content menu, Fig. 67. Step 5. With the face still selected, click Convert Entities on the Sketch toolbar. Step 6. In the Convert Entities Property Manager click OK, Fig. 68 and Fig. 69. R. Helix for Sweep Cut. Step 1. Click Insert Menu > Curve > Helix/Spiral. Step 2. In the Helix/Spiral Property Manager set: under Defined By, Fig. 70 select Pitch and Revolution under Parameters select Constant Pitch Pitch: 2.7 check Reverse direction Revolution:.98 Start angle 0 select Counterclockwise Zoom Fig. 66 Face Fig. 67 Fig. 68 Fig. 69 click OK. Fig. 70 Fig. 71 SolidWorks 13 PROPELLER DELTA DART Page 8-13

14 S. Cut Sweep Sketch Profile. Step 1. Click Top Plane in the Feature Manager and click Sketch from the Content toolbar, Fig. 72. Step 2. Click Corner Rectangle in the Rectangle flyout the Sketch toolbar. (S) on Step 3. Draw a rectangle out in front of the hub, Fig. 73. Keep the right rear corner sort of close to the right edge of the hub. Fig. 72 Fig. 73 Step 4. Right click drawing and click Select from menu to unselect Rectangle tool. Step 5. Ctrl click cylindrical converted edge and vertex of rectangle to select both. Release Ctrl key and click Make Pierce on the Content menu, Fig. 74. Make Pierce adds a Pierce relation between both sketches. Step 6. Click Smart Dimension toolbar. Step 7. Dimension rectangle 2.7 by 2, Fig. 75. (S) on the Sketch Fig. 74 Ctrl click converted edge and endpoint Step 8. Click Exit Sketch on the Sketch toolbar. Step 9. Save. Use Ctrl-S. Fig. 75 SolidWorks 13 PROPELLER DELTA DART Page 8-14

15 T. Sweep Cut Helix. Step 1. Click Features Step 2. Click Swept Cut on the Command Manager toolbar. on the Features toolbar. Step 3. In the Cut Swept Property Manager: under Profile and Path, Fig. 76 Profile box, click rectangle sketch, Fig. 77 click in the Path box and click helix expand Options uncheck Align with end faces click OK. Step 4. Save. Use Ctrl-S. Rectangle Fig. 76 U. Cut Hub. Step 1. Click Right Plane in the Feature Manager and click Sketch from the Content toolbar, Fig. 79. Fig. 77 Step 2. Click Normal To on the Standard Views toolbar. Step 3. Zoom in around hub, Fig. 80. To zoom, hold down Shift key and drag with middle mouse button (wheel). To pan, hold down Ctrl key and drag with middle mouse button (wheel). Fig. 79 Zoom Fig. 78 Fig. 80 SolidWorks 13 PROPELLER DELTA DART Page 8-15

16 Step 4. Click Line toolbar. (L) on the Sketch Step 5. Draw line from tip vertex of sweep cut to bottom sweep cut edge, Fig. 81. Step 6. Click Smart Dimension (S) on the Sketch toolbar. Fig. 81 Step 7. Add.58 dimension, Fig. 82. Step 8. Click Features Command Manager toolbar. on the Step 9. Click Extruded Cut the Features toolbar. on Step 10. In the Cut-Extrude Property Manager set: under Direction 1, Fig. 83 End Condition Through All check Flip side to cut check Direction 2 End Condition Through All The Direction arrow should point towards area to be cut away, Fig. 84. If arrow is pointing in wrong direction, unclick Flip side to cut, Fig. 83. Direction arrow Fig. 82 Fig. 84 Fig. 85 Click OK. Fig. 83 SolidWorks 13 PROPELLER DELTA DART Page 8-16

17 V. Material POM Acetal Copolymer. Step 1. Click Trimetric on the Standard Views toolbar. Step 2. Right click Material Material, Fig. 86. in the Feature Manager and click Edit Step 3. Expand Plastics in the material tree and select POM Acetal Copolymer. Click Apply and Close. W. Appearance Color. Step 1. Click the bottom blade, click Appearance Callout on the Content menu and click PROPELLER, Fig. 87. Fig. 86 Step 2. In the Appearances Task pane, expand Plastic, click High Gloss and in the lower pane select red high gloss plastic, Fig. 88. Click OK. Step 3. Save. Use Ctrl-S. Click blade Fig. 87 Fig. 88 Fig. 89 SolidWorks 13 PROPELLER DELTA DART Page 8-17