Gumball Dispenser

Step 1

Before starting on this task be reminded that if you run into difficulties, the Help window includes, a study guide, a link to Time Mechanic and thinkdesign help which includes 15 rules of Solid Modeling.

1. Open thinkdesign and open a New Model . Close the History tree.
   
2. Right click in workspace and select Options.
3. Click on the General tab and set the unit of measure to Inches and OK the dialog box.

   

4. Start the Profile Mode in the toolbar and we're ready to draw. Next select the Polyline command.

5. We'll draw the profile. View the completed profile below before you begin so you see what your final profile will look like. Select the Polyline tool and start from a point in the lower portion of your workspace. Draw a 3.5 inch vertical line up, a 4.5 inch horizontal line to your right, another vertical line down. Notice the constraints appear as you complete each line, Ve,CoY and Ho. Complete the profile with a short line to your left, a vertical line up, another horizontal line across to your left, a vertical line down and complete the profile with a short line to close it.
6. Great work. Here's the profile.

   

7. Hit any line of the profile and right click select Chain to enable the Linear Solid command.

8. Select any color and we'll sweep the profile.

9. Let's create the solid with the Linear Solid command. Set the Depth to 6.75 and hit .

   

10. Dynamically rotate and here's the sides and back of the dispenser.

    

11. Let's insert two 0.125 slots in each side of the dispenser. The slots will accept a plastic face cover (to be positioned later).
12. Place the work plane on the top and start the Parallel lines command.
13. Select Unlimited and Single lines.
14. Select one of the bottom edges and type 0.125 and hit enter.
15. Select the same line again and this time type 0.25 and again hit enter.
16. Click on the left outer edge and type 0.375 hit enter and repeat for the right side.
17. Select the Smart delete command and trim the intersecting lines leaving only a rectangle. The finished slot is surrounded by the red rectangle below.

    

18. Right click on any edge and Select, Chain from this to highlight the profile.
19. Start the Linear Slot command in the solids toolbar, select Extension Thru all and hit .

    

20. Rotate and view your slots.

21. Let's remove a section of the back to accept the bottom of the dispenser. Dynamically rotate the solid and place the work plane on the inside face of the back.
22. Start the lines command and select Parallel lines command. Set the Type to Copy length and Single.
23. Select the bottom edge of the inside face and type 1.25 and hit enter. For better visibility switch to the Wireframe command . Return to the Shaded view .
24. Change to Two-point lines command. Draw a rectangular profile by picking the endpoint of the line we just created and the bottom snap of the side edge. Continue by snapping to the other bottom edge and then back up to the other end of the parallel line. Hit Esc. to end the command.
25. Right click on the first horizontal parallel line to Select, Chain from this then, Linear Slot the profile by selecting Thru all and enter the command.

    

26. Let's create the bottom in place. Use the Parallel lines command and select the bottom inside edge of the back. Type 0.5 and hit Enter.
27. Switch to the Two-point lines command and complete a rectangular profile. For better visibility switch to the Wireframe command . Return to the Shaded view. .
28. Time to use Linear Protrusion . Select Protrusion and set the Depth to 3 and hit hit .

    

29. A pin is needed as a stop located in the center of the bottom. Select the Simple Shaft command on the solids toolbar. The shaft will have a diameter of 0.25 and a height of 0.375. In the Position tab select the top face of the bottom as the face and make the center From two edges. Set the distances at 1.5 and 1.5 to center the shaft and there it is

    

30. A hole is needed to allow the gumballs through the bottom of the dispenser. Start the Simple Hole command and set the diameter to 0.75. Tab set the center From two edges and set the distances as 3 for the first distance and 1.5 for the second distance. Select Thru all and hit .

    

31. Rotate for a better view. Good Job!

    

32. Let's give some shape to the sides. We'll accomplish this by simply adding a hole through the sides. Set the Workplane on one of the sides and start the Simple Hole command. Set the diameter to 1.25, the first distance to 1.75 and the second distance to 0, select Thru All, hit the green check and there you have it.

    

33. Hide the entities and you're off to a good start.