paper cup kho tài liệu bách khoa

Create a new sketch Ctrl +K or right click and select New Sketch.. Select Extrude Profile and set the dialog box as in figure 7.. Select Extrude Profile and extrude the two holes, subtra

Paper Cup Dispenser

Pro/DESKTOP 8

Prepared by: Harry Hawkins

Prerequisite Understanding of:

New Skills You Will Develop:

This project will provide you with exercises in creating a paper cup

dispenser You will use the normal Pro/D functions of creating workplanes and sketches as well as the duplicate and mirror functions In addition to

dimensioned views of each part included in the tutorial text, a complete set of orthographic drawings and details are included at the end of the tutorial You may refer to these drawings occasionally to verify and obtain accurate dimension numbers

Each unit of the dispenser will be constructed as a separate design and saved with its own name After all parts have been designed, they will be

assembled in an assembly design

You will also be able to produce an Album of the completed unit and experiment with various materials and features

The tutorial is presented in serial order and you should complete it by completing each step in order The numbers will continue through each part so that the entire tutorial will proceed from number 1 to the last number rather than separately number the steps for each part

Top Unit

The top unit is used to support the containment dowel rods and allow for inserting a stick of 9 oz paper cups into the holder

1 Open a new Pro/D design and edit the initial workplane under base to Top

2 Draw the outline shown in figure 1 Do not draw in the 0.25” holes yet

Figure 1 Top Unit Dimensions

3 Use Extrude Profile to extrude the design by a distance of 0.75” as in figure

2

Figure 2 Extruding the design profile

4 Select the top face of the extruded design as in figure 3 It will turn red

Figure 3 Select top face prior to creating a new sketch

5 Create a new sketch (Ctrl +K) or right click and select New Sketch Name it Holes Click OK to create the sketch

6 Use the View Orthographic Workplane (Shift +W) to view the design

7 Draw a 4” bolt circle and a vertical line from the center intersecting the bolt circle Now draw one 0.25” diameter hole at the intersection as in figure 4 Notice the bolt circle and vertical line are made into construction lines

Figure 4 Locating the first hole on the 4” bolt circle

8 Select the 0.25” Diameter hole (it will turn red) then use Ctrl +D or select Duplicate under the Edit drop down menu A duplicate menu will appear as in figure 5 Select the Circular button and enter the number 8 (the total number

of holes) Angle should be 360 and Total angle should be checked Click OK

to execute the command

Figure 5 Duplicate dialog box used to duplicate holes

9 The holes will be duplicated and should look like figure 6

Figure 6 Holes Duplicated on the 4” bolt circle

10 Rotate the view to see it in 3D Select Extrude Profile and set the dialog box

as in figure 7 Subtract material below the workplane a distance of 0.25” Click OK to execute the command

Figure 7 Removing material to create holes

11 Your design should look like figure 8

Figure 8 Holes completed in Top Unit

12 Use edge selection to select the top and bottom edges of the design (do not select the back edges) Use Shift to select more than one edge

13 With the edges selected, right click and select round edges Use 0.125” as the Radius Click OK to complete the round

14 In a similar fashion, select the top and bottom edges of the center hole and round these edges to 0.125” as well The design should now look like figure 9 Rotate it and view it from various angles

Figure 9 Rounds completed

15 Rotate the image so that you can see the rear face Use face selection and select the rear face Right click and create a new sketch Name it Top

Mounting Holes

16 Using the dimensions in figure 10, place the two R=0.063” Mounting holes in the new sketch Be sure to delete locating lines or change them into

construction lines so that you will have a valid profile

Figure 10 Layout for mounting holes

17 Select Extrude Profile and extrude the two holes, subtract material below the workplane a distance of 0.5” as shown in figure 11 Click OK to execute the extrusion and create the mounting holes

Figure 11 Extrude Profile for mounting holes

18 The top unit is now be finished It should look like figure 12 Revolve it to view it from various angles then save it as Top Unit

Figure 12 Completed Top Unit in transparent mode for clarity

Bottom Unit

The bottom unit is largely the same as the top unit that you have just

completed One important difference is that the hole through the bottom unit

is tapered so that the paper cups will be held lightly and so you can pull one cup from the stack without all the cups coming out

19 Open a new Design in Pro/D

20 Use the dimensions in figure 13 to layout the bottom unit profile Do not draw the center hole or dowel rod holes at this time

Figure 13 Dimensions for bottom unit profile

21 Use Extrude Profile to extrude the profile a distance of 0.75” above the

workplane as shown in figure 14 Press OK to execute the extrusion

Figure 14 Extruding the bottom profile

22 Select the top face of the completed profile (it will turn red) Right click and select New Sketch Name the sketch bottom center hole Click OK to create the new sketch

23 Draw the 3.375” circle at the appropriate place on the profile such as shown

in figure 15

Figure 15 Creating bottom unit center hole profile

24 Select Extrude Profile and edit the dialog box according to figure 16 Notice that material is to be subtracted a distance of 0.75” below the workplane and also at a 6 degree taper Notice a yellow trial view of the extrusion Press OK

to execute the extrusion

Figure 16 Creating the tapered center hole in the bottom unit

25 Select the top face again (it will turn red), right click and create a new sketch Name the sketch bottom dowel holes View the drawing in orthographic and locate and draw in one 0.25” diameter hole on a 4” bolt circle as shown in figure 17

Figure 17 Inserting first dowel rod hole

26 Select the hole just drawn (it will turn red) then select Duplicate (under the View Menu) Complete the dialog box as shown in figure 18 Click OK to duplicate the holes

Figure 18 Duplicating the dowel pin holes

27 The dowel holes should be duplicated equally around the 4” bolt circle Figure

19 shows the completed duplication

Figure 19 Holes duplicated

28 Select Extrude Profile and complete the dialog box as in figure 20 You will

be subtracting material below the workplane a distance of 0.5” Click OK to execute the command

Figure 29 Extruding the dowel pin holes

29 The design should look like figure 21

Figure 21 Bottom Unit with dowel pin holes completed

30 Rotate the image to see the back face Use face select to select it (it will turn red) then right click and select New Sketch Name the sketch bottom

mounting holes as in figure 22 Click OK to create the new sketch

Figure 22 Create new sketch for mounting holes

31 Display the new sketch in orthographic and locate and place two holes of R=0.063” according to figure 23 After inserting the first hole, select it (it turns red) then hold the shift key down when you drag the second hole It will automatically be the same diameter as the first Be sure to delete locating lines or change them into construction lines so that you have a valid profile

Figure 23 Layout for mounting holes

32 With the two hole profile completed, select Extrude Profile Set the dialog box according to figure 24 Notice a trial visual in yellow Click OK to execute the extrusion

Figure 24 Extrude Profile dialog for mounting holes

33 Select all edges except the rear face edges and round them to 0.124” Use the shift key to select multiple edges then right click and select round edges and set the radius to 0.125” then press OK to execute the rounds Figure 25 shows all rounds completed This completes the bottom unit Save it and give

it the name “Bottom Unit”

Figure 25 Completed Rounds

34 The bottom unit is now complete It should look like figure 26 If you have not already done so, save this design and name it Bottom Unit

Figure 26 Completed bottom unit viewed as transparent for clearer view of holes

Back Board

35 Start a new design Construct the part-profile shown in figure 27 Notice this

is the right half of the back board Draw a construction line then the right side line first Make the center line fixed so it will not move Use the Spline (B) tool to construct the curves at the top of the unit This is done by eye

Figure 27 Mirroring the curves from the top to the bottom

36 Once the top curves are drawn, create a horizontal center construction line This will be the axis for the mirror function

37 Under Line, select Mirror The mirror sketch lines dialog box will appear as

in figure 28 Select the lines to be mirrored – in this case the curved lines You can use a selection box to select all lines

Figure 28 Curved lines selected to me mirrored

38 Now click on the Axes tab then select the horizontal line used as the mirror axis A visual image of the mirrored line will appear at the bottom as in figure

29 Click OK to execute the mirror

Figure 29 Mirror image ready to be completed

39 Use the delete line segment function to remove unwanted lines including the horizontal axis used for the previous mirror

40 Under Lines, select Mirror This time select all the lines except the vertical construction line at the left then click the Axis tab and select the vertical construction line The mirrored view will be visible to the left as in figure 30 Click OK to execute the mirror The unit should turn color indicating a valid profile

Figure 30 Mirroring the left side of the image

41 Move the image so it will be viewed in 3D then select Extrude Profile Set the dialog box according to figure 31 with adding material above the workplane a distance of 0.25” Click OK to execute the extrusion

Figure 31 Extruding the back board profile

42 Use select faces to select the top face of the image (it will turn red) Right click and select New Sketch Name the sketch wall mount holes as in figure

32

Figure 32 Creating the sketch for the two wall mounting holes

43 Layout and insert a 0.125” diameter hole at the top of the image according to figure 33 This will be a temporary hole to locate the place where a custom counter sunk hole will be inserted

Figure 33 Locating a hole for mounting on the wall

open such as in figure 34 Select Counterbore, Extend Thru entire part and the C’bore diameter = 0.375”, hole Diameter = 0.125” and C’bore depth = 0.125” Click OK to install the hole

Figure 34 Dialog box setup to install Counterbore hole

45 The completed hole should look like figure 35 Note that this view has been rotated to see it in 3D and to more clearly show the counterbore

Figure 35 Counterbore hole installed

46 Draw a horizontal construction line at the midpoint of the image This will serve as an axis for duplicating the counterbored hole

47 Under Line, select mirror Select the center hole in the countersunk feature then select the Axis tab and select the horizontal axis The mirrored hole will show as in figure 36 Click OK to complete the mirror

Figure 36 Bottom counterbored hole installed my mirroring

48 We will now install mounting holes for the top and bottom units First we will install a hole for the top then use mirroring to place the other three holes

49 Rotate the image so that the rear face is visible Select the rear face then right click and select New Sketch Name the sketch unit mounting holes

50 Locate and install a R=0.063” hole 3.60” down from the top and 1.375” to the right according to figure 37 Be sure to delete any construction lines

Figure 37 Installing first top unit mounting hole

51 Select the hole then select Insert holes Complete the dialog box as in figure

38 This time we will use a standard 8-32UNC countersink hole By selecting

a standard size, all the dimensions for the countersink are automatically inserted Click OK to insert the hole

Figure 38 Inserting the first 8-32UNC Countersunk hole

52 Draw a vertical and a horizontal construction center line These will be used

to mirror the countersunk hole

53 Under Line, select mirror then select the center hole just drawn Select the vertical construction line as an axis and OK to mirror the top left hole

54 In a similar fashion, select both top holes and use the mirror function to select the horizontal axis to place the two bottom holes The finished back board with these 4 holes inserted is shown in figure 39 This is a view from the back of the board

Figure 39 Support unit countersunk holes installed

55 This completes the back board Rotate it to view it from various angles Save

it and name it Back board

Dowel Rod

We will create 1 dowel rod and install it a total of 8 times in the final

assembly This is a relatively easy design that can be done quickly

56 Open a new design and draw a 0.25” circle as shown in figure 40

Figure 40 Dowel rod profile

57 Rotate the profile to see it in 3D then select Extrude Profile You will add material below the workplane a distance of 10.565” Click OK to complete the extrusion It should look like figure 41

Figure 41 Completed Dowel Rod

58 This completes the dowel rod Rotate it and view it from different angles then save it Name it Dowel Rod

0.0120

Ø0.0900 Ø0.0500

60 Figure 44 is a detailed dimensioned view of the fold at the lower right edge

Figure 44 Detailed dimensions for the cup bottom fold

61 Draw a vertical line of 3.53” Make it a construction line Now draw a

horizontal line from the top of this line to the right a distance of 1.551” Draw

a horizontal line from the bottom of the construction line to the right a distance of 1.025” Figure 45 shows these details

Figure 45 Starting lines for cup profile

62 Zoom in on the top right corner where the profile for the rolled lip will be and construct the two circles as shown in figure 46 Draw a 0.045” vertical construction line to locate the circle centers (see figure 43)

Figure 46 Forming the rolled lip

63 At the lower edge of the center construction line, construct the two lines shown in figure 47 The curves and radii dimensions shown are approximate They may be slightly different than the illustration The thickness is 012” (see figure 44)

Figure 47 Details of bottom profile layout

64 Figure 44 shows the detail of the lower right edge Note that the small

horizontal line at the bottom is not a curve but a short straight line See figure 44 for correct dimensions

65 Connect lines from the bottom of the base fold tangent to the circles of the rolled lip Delete segments of the lip circles such as in figure 43 Delete all unwanted lines or make them construction lines and be sure you have a filled profile such as shown in figure 48

Figure 48 Filled profile ready for revolve

66 In order to execute a revolve profile function; you must have two sketches on one workplane We already have the cup profile on the initial workplane We now need to create an axis on a new sketch

67 Under the Workplane drop-down menu select New Sketch (Ctrl +K) Name the new sketch Axis and make sure it is added to the base workplane Click

OK to create the sketch

68 Draw a vertical line from the left bottom to the left top as shown by the arrow

in figure 49

Figure 49 Axis line drawn at left of profile

69 Orient the image for 3D viewing then select Revolve Profile A dialog box will appear Complete the dialog box according to figure 50 Be sure that initial is

in the Sketch to use as profile box If it is not select the box arrow button and select it Click on the Axis button and then double click the axis line in the design until it turns red Return to the Revolve Profile dialog and click

OK to complete the revolve

Figure 50 Revolve profile ready to be executed