Assignment 4: Make A Molecule

Introduction

Using a free, open source molecule editor like Avogadro you can construct your own molecular models, solve for low-energy configurations, and read out the bond lengths and bond angles. But for this assignment we've done all that work for you. All length values given in "inches" below are really in picometers, and all bond angles are physically accurate.

In this assignment you will construct an ethanol molecule in SolidWorks that is hollow inside and has a removable threaded cap. You will then 3D print the molecule and the cap.

Making the Cap

1. Start a new part.
2. Create an extruded base on the Top Plane
3. Draw a circle centered on the origin and dimension the diameter to 2.1 inches
4. Set the extrude depth to 0.75 inches.
5. This creates a disk.

6. Create a Revolved Base feature on the Right Plane.
7. Draw a horizontal line along the top edge of the disk, starting at the midpoint (directly above the origin) and running leftward to just past the edge of the disk.
8. Dimension the horizontal line to 1.2 inches.
9. Draw a vertical line upward from the top edge of the disk, rising from the midpoint.
10. Add an Equal relation between the two lines.
11. Draw a 90 degree centerpoint arc connecting the ends of the two lines. To assure that the arc merges properly with the line endpoints, follow these steps:
    1. Select the Centerpoint Arc tool
    2. Click on the point where the two lines meet; that will be the arc center.
    3. Click on the top of the vertical line.
    4. Move the mouse down and to the left to form an arc, but stop before reaching the horizontal line.
    5. Press Escape to exit the arc tool.
    6. Click on the bottom endpoint of the arc.
    7. Control-click on the left endpoint of the horizontal line.
    8. Select "Merge" in the Property Editor to merge the two endpoints.
12. Exit the sketch and use a 360 degree revolve of the quarter circle around the vertical line to form a hemisphere.

13. Click on the flat bottom of the cap to select it.
14. Use the Shell feature to hollow out the cap; set the shell thickness to 0.2 inches.

15. Save your part as Cap.SLDPRT

Threading the Cap

CUTTING PROFILE

1. In this step we'll make an equilateral triangle to cut threads in the lip of the cap.
2. Make a new sketch on the Front plane.
3. Draw a vertical line about 0.2 inches long, somewhere below the bottom left edge of the lip. The exact length and position aren't important.
4. Draw a diagonal line starting at the top of the vertical line and moving down and to the right, with about the same length as the vertical line.
5. Add a third diagonal line to complete the triangle.
6. Add an Equal relation between the two diagonal lines.
7. Dimension the angle between the two diagonal lines to 60 degrees.
8. Draw a vertical construction line connecting the midpoints of the diagonal lines.
9. Dimension the construction line to length 0.1 inches.
10. Click on the vertical line.
11. Control-click on the left vertical edge of the cap lip. (There may not appear to be a line there, but click on the edge and a silhouette edge will appear.)
12. Add a Colinear relation.
13. Click on the point where the two diagonal lines meet.
14. Control-click on the bottom edge of the cap lip.
15. Add a Coincident relation.
16. Now the sketch should be fully defined (black).
17. Click OK to exit the sketch.

    CUTTING PATH

18. Now we'll make the helical path that the cutting sketch will follow.
19. In the Features tab, open the Curves pulldown menu and select "Helix and Spiral".
20. Select the bottom face of the cap lip (the very bottom of the cap) as the plane for your sketch.
21. Use a Normal To view so the cap edges form perfect circles.
22. Select the outer edge of the cap lip. (This will be the middle of three visible circles.)
23. Click Convert Entities to copy the circle into the current sketch.
24. Click OK to exit the sketch.
25. In the Helix/Spiral property manager, select a constant pitch of 0.25 inches.
26. Set the revolutions to 3 and check the Reverse direction box so that the yellow spiral ascends into the cap.
27. Set the Start angle to 270 degrees to ensure that the start of the helix coincides with the location of the triangular profile sketch. (If you layed things out slightly differently you might need a different start angle.)
28. Click OK to complete the helix.

    

    THREAD FEATURE

29. In the Features tab, select Swept Cut.
30. Open the feature tree in the top left corner of the graphics area.
31. For the sweep profile (blue box), select the triangular profile sketch.
32. For the path (pink box), select the Helix/Spiral feature.
33. Click OK to complete the feature.

34. Save your part as Cap.SLDPRT
35. Then do "Save As" and set the file type to STL. In the save dialog box, click on the Options button and select Fine resolution.
36. Save the file as Cap.STL.

Making the Molecule

1. Create a new part.

   FIRST CARBON:

2. Create a Revolved Base Feature, sketching on the Top Plane.
3. Draw a vertical line extending THROUGH the origin and dimension it to length 3.4 inches.
4. Select the line's midpoint and make it coincident with the origin.
5. Use the centerpoint arc tool to draw a left semicircle bounded by the vertical line endpoints:
   1. Select the centerpoint arc tool.
   2. Click on the origin; that is your centerpoint.
   3. Click on the top point of the vertical line.
   4. Move the mouse down and to the left, approaching but not touching the bottom point of the vertical line.
   5. Left click to draw the arc.
   6. Select the arc endpoint.
   7. Shift click on the bottom point of the vertical line.
   8. Click on Merge in the properties tab.
6. Exit the sketch and use a 360 degree revolve of the semicircle around the vertical line to form a sphere.
7. In the Feature Manager Tree, rename the feature Carbon1.
8. Color the entire sphere (the Carbon1 element in the Appearances pop-up list) pale green.

   SECOND CARBON:

9. Create a new sketch on the Front Plane.
10. Draw a vertical construction line upward from the origin and dimension it to 1.54 inches.
11. Exit the sketch.
12. In the Feature Manager Tree, rename the sketch to Backbone1.
13. Create a Linear Pattern feature and set the vertical line of Backbone1 as Direction 1.
14. Set the distance D1 to 1.54 inches.
15. Set the # of instances to 2.
16. Set the Revolve feature as the Features to Pattern (just click on the sphere to select it).
17. If the Reverse direction button (to the left of the Direction 1 box) is selected, click it to deselect. We want the yellow outline of the new carbon being constructed by the linear pattern to be on the same side as the dashed Backbone line. (If you don't see a yellow outline, click on "Full Preview" in the linear pattern dialog box on the left.)
18. Click OK.
19. Rename the feature Carbon2.

    FIRST HYDROGEN:

20. Create a new Revolved Base on the Front Plane.
21. Draw a diagonal construction line from the origin downward and to the left.
22. Dimension the line length to 1.1 inches.
23. Dimension the angle between the line and the vertical Backbone line from the previous sketch to 109 degrees.
24. Draw a new vertical line (solid, not a construction line) through the bottom left endpoint of the line you just drew.
25. We want the midpoint of the new vertical line to be coincident with the left endpoint of the diagonal line, so add a relation to enforce this property.
26. Dimension the line to length 2.4 inches.
27. Use the centerpoint arc tool to draw a semicircle to the left of and bounded by the vertical line. Merge the second endpoint.
28. Exit the sketch, and in the Revolved Base dialog box, make sure that the axis of revolution selected is the solid vertical line, not the diagonal construction line. Use a 360 degree revolve of the semicircle to form a sphere.
29. Note: if there is a problem with your sketch and SolidWorks wants to make the Revolved Base a "thin" feature, cancel the feature and then edit the sketch. Once a feature is marked "thin" there does not appear to be a way to undo this, and a thin feature is not suitable here. One possible cause of this problem is if the vertical line was made a construction line instead of a solid line.
30. In the Feature Manager Tree, rename the Reolved Base feature to Hydrogen1.
31. Color the sphere (Hydrogen1 in the Appearances pop-up list) white.

    SECOND AND THIRD HYRDROGENS:

32. Create a Circular Pattern feature (in the pulldown menu from Linear Pattern).
33. For the axis/surface of rotation parameter (first box in the "Parameters" section), select Backbone1.
34. For the # of instances, select 3.
35. Check the Equal Spacing box.
36. For the Features to Pattern, select Hydrodgen1.
37. Click OK to complete the feature.

    OXYGEN:

38. Make a new Revolved Base on the Front Plane.
39. Draw a diagonal construction line from the top end of the Backbone line up and to the right, and dimension it to length 1.43 inches.
40. Set the angle between the vertical and diagonal construction lines to 120 degrees.
41. Draw a solid horizontal line centered on the endpoint of the diagonal construction line, and dimension is to length 3.04 inches.
42. Select the midpoint and add a relation to enforce this property.
43. Use the centerpoint arc tool to draw a semicircle above the horizontal line.
44. Merge the second endpoint.
45. Exit the sketch and make sure that the axis of revolution is the solid horizontal line, not the diagonal construction line. Use a 360 degree revolve of the semicircle to form a sphere.
46. Rename the feature to Oxygen1.
47. Color Oxygen1 red.

    FOURTH HYDROGEN:

48. Go the Features Tab, and in Reference Geometry, create a Plane.
49. Set the first reference to Top Plane
50. Set the second reference to the top point of your Backbone line and click OK.
51. Rename the plane Carbon2Plane.
52. Create a new Revolved Base feature on Carbon2Plane.
53. Draw a horizontal construction line from the origin to the left.
54. Draw a diagonal construction line from the origin up and to the left, and dimension it to 1.1 inches.
55. Set the angle between the two construction lines to 70 degrees.
56. Draw a solid horizontal line with its midpoint being the top point of the diagonal construction line.
57. Add a relation to enforce the midpoint constraint.
58. Dimension the horizontal line to length 2.4 inches.
59. Use the centerpoint arc tool to draw a semicircle above and bounded by the horizontal line. Merge the second endpoint.
60. Exit the sketch and use a 360 degree revolve of the semicircle to form a sphere.
61. Rename the feature Hydrogen4.
62. Color Hydrogen4 white.

    FIFTH HYDROGEN

63. Create a mirror feature.
64. Set the mirror face/plane to the Front Plane.
65. Select Hydrogen4 as the feature to mirror.
66. Click OK to complete the mirror.

    SIXTH HYDROGEN

67. Create a Revolved base on the Front Plane.
68. In the Feature Manager Tree, expand the Oxygen1 feature to reveal its sketch.
69. Right click on the sketch and click "Show" (the eyeglasses icon) to make it visible.
70. Add a new construction line from the end of the oxygen diagonal line, running almost vertically but slightly to the right.
71. Dimension this construction line to 0.94 inches and set the interior angle between it and the diagonal below the horizontal line to 125 degrees.
72. Draw a solid horizontal line centered on the new construction line, and dimension is to length 2.4 inches.
73. Use a midpoint relation to ensure that the horizontal line is centered properly.
74. Use the centerpoint arc tool to draw a semicircle above the horizontal line.
75. Merge the second endpoint.
76. Exit the sketch and use a 360 degree revolve of the semicircle to form a sphere.
77. Rename the feature Hydrogen6.
78. Color the sphere white.

    CAP OPENING:

79. In the Features tab, under Reference Geometry, create a new Plane.
80. For the first reference, hover the mouse over the boundary circle where Hydrogen6 meets Oxygen1. The boundary should be highlighted in orange. Click to select it.
81. The plane is now fully defined; click OK to exit.
82. Rename the plane to Hydrogen6Plane.

83. Create an Intersect feature. If you don't have the icon for Intersect (it's not visible by default), open the slide-out menu at the top of the window and select Insert -> Features -> Intersect
84. In the Selections box, add both Hydrogen6Plane and Hydrogen6.
85. Click on the Intersect button. The entire molecule should turn green.
86. Now we need to specify regions to exclude. Click on on the Hydrogen6 sphere in the graphics window (not the feature in the feature manager tree); it should turn pink.
87. Cllick OK to complete the Intersect operation.
88. Right click on Hydrogen6Plane in the feature tree and hide it.

    SHELL:

89. Click on the flat surface at the top of the Oxygen1 sphere.
90. Create a Shell feature.
91. Set the shell thickness to 0.2 inches.
92. Click OK to complete the shell.
93. Save your part as Ethanol.SLDPRT

Threading the Molecule

LIP:

1. Create an Extruded Base feature on the flat lip of the opening in the Oxygen1 molecule.
2. In the sketch editor, click on the inner circle of the Oxygen molecule opening.
3. Click on Convert Entities to import that circle into the sketch.
4. Reselect the same inner circle and click on Offset Entities to create a slightly bigger circle outside it.
5. Set the offset distance to 0.2 inches and click reverse if necessary to make sure the new circle is outside the inner circle. Click OK.
6. Click OK to accept the sketch.
7. Set the extrusion depth to 0.75 inches.
8. Adjust the direction (the button with the arrows to the left of the "Blind" menu setting) so that the extrusion extends into the molecule's interior.
9. Click OK to complete the extrusion.
10. Rename this feature Lip.

    

    CUTTING PROFILE:

11. In the feature manager tree, open Hydrogen6, right click on its sketch, and select Show to make it visible.
12. Make a new sketch on the Front plane.
13. When you select a Normal To view, notice that the lip in Oxygen1 is tilted slightly down and to the right. That's fine.
14. Above the lip in Oxygen1, near its left edge, draw a vertical line about 0.24 inches high that isn't snapped to any other feature.
15. Form a triangle by adding two diagonal lines to the left of the vertical line.
16. Add an Equal relation between the two diagonal lines.
17. Dimension the angle between the two diagonal lines to 60 degrees.
18. Add a construction line connecting the two midpoints of the diagonal lines.
19. Dimension the construction line to length 0.12 inches. The result should look like this:
20. Click on the solid vertical line and remove its Vertical property.
21. Click on the construction line and remove its Vertical property as well.
22. Click on the solid vertical line, shift click on the circular edge of the lip, and add a Perpendicular relation between them. This should tilt the triangle slightly upward, matching the lip.
23. Click on the point at apex of the triangle (the leftmost point), and shift click on the circlular edge of the lip.
24. Add a Coincident relation between the point and the circle.
25. Dimension the distance between the formerly vertical solid line and the near-vertical construction line in the Hydrogen6 sketch to 0.925 inches.
26. Now the triangle should be fully defined (black).
27. Click OK to exit the sketch.
28. Hide the Hydrogen6 sketch.

    CUTTING PATH:

29. In the Features tab, open Curves and create a Helix and Spiral feature.
30. Select the flat face of the Oxygen6 opening as the sketch plane.
31. Click on the circle that forms the inner edge of the lip.
32. Click on Convert Entities to import the circle into this sketch.
33. Click OK to complete the sketch.
34. Set the helix pitch to 0.25 inches and the number of revolutions to 3.5.
35. Set the Start angle to 0 so that the yellow line in the preview begins at the triangle that forms the cutting profile.
36. The spiral should extend down into the red oxygen molecule; if it's extending upward, click on the Reverse Direction box in the Helix/Spiral dialog pane.
37. Click OK to complete the helix.

    

    THREAD FEATURE:

38. In the Features tab, select Swept cut.
39. Click on the triangle to select it as the proflie (blue box).
40. Click on the helix to select it as the path (pink box).
41. Click OK to complete the feature.

    BASE:

42. Add an extruded base of your own design to the bottom of the molecule that can act as a stand. See the figure below. We used three cylinders in our design, but you are free to innovate. Add your initials or some other unique feature to distinguish your molecule from others.

Preparing to Print on the Cube 3

The molecule must be printed with the threads flush with the print bed, since there are no internal supports for the threaded lip. Thus, the molecule needs to be flipped to an upside-down position and then tilted a few degrees so that the lip of the opening lies flat against the print bed. Again, a raft is required to keep the molecule from falling over during the print.

The molecule and cap can be printed at the same time. To get the raft: in the Cube Client, click on the settings button (gear icon), select Custom, and turn on the raft, but turn off supports.

Scale both parts to 40% for a quick but functional print. You can try a larger size if you're willing to spend the time and plastic. You can use fast mode (200 micron layers) even at 40%; it's not necessary to use the more precise 70 micron setting, although the results will be smoother if you're willing to wait three times longer for the print to complete.

What to Hand In

• Bring your molecule to class to show off.
• Post a picture of it on Piazza, in the thread provided.
• Hand in your SolidWorks parts files via Autolab.

Grading

• 4 points for a correct Molecule body in SolidWorks
• 1 point for a correct molecule cap in SolidWorks
• 1 point for a good stand design in SolidWorks
• 4 points for a complete printed molecule and cap with working threads, with a picture posted to Piazza

Last modified: Thu Feb 4 01:18:07 EST 2016