SolidWorks Intro Part 1

Starting Up

1. Log in using your Andrew ID.
2. Search for and run program: "Solidworks 2016 x64 Edition"
3. Turn off Simulation.

First Time With SolidWorks

1. Use IPS as default units
2. New part
3. If the SolidWorks Resources fly-out menu is visible on the right side, click in empty space in the graphics window to collapse it.
4. Turn off Instant3D.
5. Extruded base.
6. Select front plane.
7. Select corner rectangle tool.
8. Note the different types of rectangle tools available; stick with the default.
9. Move mouse and note snap-to lines above or beside the origin.
10. Draw a rectangle away from the origin, about 1.5 in wide by 1 in high.
11. Note the rectangle tool is still active.
12. Green checkmark to confirm, or escape to exit the rectangle tool.
13. Click on the polygon tool.
14. Draw a hexagon lying entirely inside the rectangle.
15. Notice the snap-to lines as you move the mouse.
16. Hit escape to exit the polygon tool.

17. Look in the top right corner for the Exit Sketch icon.
18. Click on Exit Sketch.
19. Now we've popped back to the Boss-Extrude dialog.
20. Change the depth to "1/8 in", which matches our material.
21. Look in the top right for the green OK checkmark, and click it.

22. Look at the Feature Manager Tree:
    • The root is Part1.
    • Notice the Boss-Extrude1 feature.
23. Mouse buttons:
    • Left click on a face to select the feature and bring up a shortcut menu.
    • Left click in empty space (or hit Escape twice) to deselect.
    • Scroll wheel to zoom.
    • Middle button to rotate about screen-x and screen-y.
    • Alt-middle button to rotate about screen-z.
    • Control-middle button to translate.

24. COMMON MISTAKE:
    • Use the scroll wheel to zoom WAY past the part so you can't see it.
    • Rotating won't help.
    • Scrolling won't help if you don't know which way to go (in or out).
    • Type "f" to fit the part in the window. Easy fix!
    • Or click on the "zoom to fit" icon at the top of the screen.

25. Let's go back and edit the sketch again. Three ways to do it:
    • i) Left click on a face.
    • ii) Left click on the feature in the Feature Manager tree.
    • iii) Open the feature (click on the "+" sign) and click on the sketch icon that will appear below it.
    • All of these bring up a shortcut menu.
    • Select the edit sketch icon from the menu.
    • Type a <space> to get the views menu and select "normal to".

26. DO THIS ONCE:
    1. Right click on a blank spot in the Sketch toolbar to get a pop-up menu.
    2. Click on "Customize" at the bottom.
    3. Go to the Commands tab.
    4. Click on Standard Views.
    5. Click and drag the "Normal To" tool to the sketch toolbar.
    6. Click OK to close the Customize window.

       You can also use control-8 as a keyboard shortcut for Normal To, or hit Space to get a list of view options.

27. Back to editing our sketch:
28. Click "Normal To" or type control-8.
29. Click on the right vertical line.
30. Look at the properties tab.
31. Select the "Vertical" relation and delete it.
32. Grab the top right point and drag it; now we have a quadrilateral.
33. Control-Z to undo.
34. Control-Y to redo.
35. Escape to exit.
36. Click on the Exit Sketch icon.

37. Rotate the part so you can see the corner edges.
38. Switch to the Features tab.
39. Click on the top right edge and select the Fillet tool.
40. Turn on Full Preview if it's not already on.
41. Set fillet radius to 0.05 in.
42. Add the bottom left edge, but not the other two edges.
43. Click on a FACE to see what happens. Click again to de-select.
44. Click the green checkmark to accept.

45. Look in the Feature Manager tree and see two features: Extrude1 and Fillet1.
46. Create a new fillet feature for the top left and bottom right corners; set the radius to 0.5 in.
47. Click on a face and select the Appearances icon.
48. In the appearances pop-up menu, click on the part name.
49. Select a color from the pallette and click OK.
50. Grab the rollback bar and roll back the two fillets.
51. Then roll it down again to bring back the fillets.

    DIMENSIONING

52. Edit the sketch again.
53. Click on the Smart Dimension tool.
54. Select the left vertical line and set its length to 1 inch.
55. Select the bottom horizonal line and set its length to 1.6 inches.
56. Select the right line and then the top line, and set their angle to 75 deg.
57. Select the circle inside the hexagon and set its diameter to 0.3 inches.
58. Escape to exit the Smart Dimension tool.

    RELATIONS

59. Edit the sketch again.
60. Click Normal To.
61. Click on the left vertical line; observe the Line Properties.
62. Shift-click on the right vertical line; now two lines are selected.
63. Click on the Equal relation.
64. Observe the error, then click on the OK checkmark in the property editor.
65. Click on the left vertical line.
66. Click on its Vertical property and hit Delete to remove it.
67. Click OK to accept the sketch. Looks nice!
68. Edit the sketch again.
69. Click Normal To.
70. Drag the bottom left point to the origin.
71. Notice that the parallelogram has turned black. No lines are draggable.
72. The parallelogram is now "fully defined".

73. Click on the plus sign at the center of the hexagon and drag it back inside the parallelogram.
74. Click on the top line of the hexagon.
75. Give it the Horizontal property.

    MORE DIMENSIONS

76. Click on the Smart Dimension tool.
77. Click on the point at the center of the hexagon, then on the bottom line.
78. Set the distance to 0.48 inches.
79. Escape to exit.
80. Click on the Smart Dimension tool again.
81. Click on the point at the center of the hexagon again.
82. Now click on the origin point.
83. Slide the mouse around and watch the dimension change type.
84. Bring the mouse between the two points and well above or below them to get a horizontal dimension.
85. Set this dimention to 0.6 inches.
86. Now the sketch is fully defined.
87. After you've completed a dimension, you can click and drag to reposition it.
88. Click Exit Sketch.
89. Click on File -> Save As and save your part as MyFrob.SLDPRT.

    KEYRING HOLES

90. Edit the sketch again.
91. Use the circle tool to make a small circle in the bottom left corner of the object.
92. Dimension this circle to a diameter of 0.125 inches.
93. Make another circle in the top right corner of the object.
94. His escape to exit the circle tool.
95. Click on the first circle, shift click on the second, and make them Equal.
96. Use the smart dimension tool to set the diagonal distance between the center of the bottom circle and the origin to 0.25 inches.
97. Hit escape to exit the smart dimension tool.
98. Click and drag on the center of the circle and note that it is constrained to move along an arc. Position it as symmetrically as you can.
99. Smart dimension the top circle to a diagonal distance of 0.25 inches from the top right corner.
100. Exit the sketch to see the hole placement.

     TEXT OBJECTS

101. In the Features toolbar, select Extruded Cut.
102. Click on the front face of the part and select a normal view.
103. In the Sketch toolbar, click on the text tool (capital "A").
104. Click where you want to place your text (you won't see anything yet).
105. Click in the white Text box and type your initials.
106. Click on the green checkmark.
107. Now you see a little blue dot at the bottom left corner of your text.
108. Click and drag the dot to position the text.
109. Double click on the text to re-open the text dialog box.
110. Uncheck "Use document font", click the Font button, and select a font you like.
111. Switch the font size to Points and select the size you want.
112. Click the green checkmark to exit the text dialog.
113. Click on Exit Sketch.
114. In the Extruded Cut dialog, set the cut depth to 0.01 inches and click the green checkmark.
115. In the Feature Manager tree, click on the Cut-Extrude feature, select the beach ball, and color the feature (not the entire part) orange.