Reference no: EM133748529

Laboratory Work

Laboratory work forms an essential part of the Unit, and as such, students are expected to complete and submit the reports on time.
Universal joints description

A universal joint is a type of mechanical instrument used in many applications to transmit rotation through slightly misaligned shafts (See Figure 1). The misalignment correction is limited by the design of the shaft but can be amplified by use of multiple universal joints. (1)

Typical applications of universal joints include aircraft, appliances, control mechanisms, electronics, Instrumentation, medical and optical devices, ordnance, radio, sewing machines, textile machinery and tool drives.

Universal joints are available in steel or in thermoplastic body members. Universal joints made of steel have maximum load-carrying capacity for a given size. Universal joints with thermoplastic body members are used in light industrial applications in which their self-lubricating feature, light weight, negligible backlash, corrosion resistance and capability for high-speed operation are significant advantages.

Lab Report

Students are required to document each project in the form of a lab report. The format of the Lab Report is as follows (Following the MIT format as discussed in the lectures). Use this as guideline in documenting your projects. Not all items may be needed in documenting the projects you undertake.

Purpose/Objective(s) Why are we doing the lab? What questions are you trying to answer?
Hypothesis What do you expect the results to be?
This should relate directly to the problem
Materials List of all the Materials you will use during the lab
Procedure Steps should be listed and numbered.
Steps should be clearly written, detailed, and brief
It must indicate HOW data will be taken
Tabulated Data Must be in the form of a table
Be sure to use units
Analysis Graphs, calculations, important observations
Conclusion A good conclusion answers 3 questions:
What did you do in the lab?
Restate the purpose/problem
A brief description of how you tested it
What you used to gather data
What does your data say?
Look at your data table or sketch and turn it into a sentence or two.
What did you learn?
This should answer the question posed in the purpose/problem.

Part 1: Drawing One Eye End

In order successfully complete this lab, you need to carefully read and follow every step of the instruction.
Objective: To draw 3D model parts of Universal Joint and join them together in full assembly
Materials Required:
Solidworks Software
Procedure:
Start-up Solidworks software and create a new document from File menu, select Part from Templates and click OK. The units to be used are millimeters.
Select Front Plane, click sketch.
Draw the rectangle starting from origin using center rectangle with the width of 60 mm and height 90 mm.

Go to Features tab, extrude rectangle to 15 mm.

Select the following top face and click sketch.

Draw 2 circles with same origin of diameters of 30 and 60 mm.

Under smaller circle in the center draw corner rectangle to the right with the size of 3 and 4 mm as shown below.

Expand Trim Entities and select Extend Entities tool, select right side of rectangle and drag it upwards till the edge of smaller circle (it will extend right side line upwards until circle's edge).

Select Trim entities and trim inside lines.

Using tool mirror Line 3 and Line 4 about Line 2 (you may have different numbering) as follows.

Select Trim entities and remove lines between smaller circle and rectangle as shown below.

Go to features tab, click on and extrude that part to 30 mm.

Select the following top face, click sketch and normal to.

Draw the following two circles with same origin of size 16 and 46 mm, vertically aligned with main origin . Set the distance from circles' origin to the lower side of rectangle to 35mm as follows.

Using Line, draw the following 2 lines (one line across top edge of rectangle and other line from right end to the middle right part of larger circle

Draw 1 more line from left corner of rectangle to the circle'edge om the left side.

Select line on the left side and while keeping CTRL key pressed select the edge of larger circle, new Properties window will appear, under Add Relations click to tangent .
-Repeat the procedure on the right side.

Add vertical relation between circle's origin and main part origin (Select circle's center point, while pressing mouse select , under Properties choose Vertical).

Select Trim Entities and remove inside lines as follows.

Go to Features tab, click Extruded Boss/Base, extrude the part to 15 mm(reverse direction)

Select Top Plane, click Mirror , select last Extruded part and press .

Save the part in New folder and name the file part1.

Part 2: Drawing Cross bearing

Create a new document from File menu, select Part from Templates and click OK. The units to be used are millimeters.
Select Top Plane, click sketch.
Draw 2 circles with diameter sizes of 30mm and 16mm.

Go to Features tab and extrude the circle to 60mm, under direction1 choose Mid Plane and press .

Select right plane, click Sketch, draw 2 circles with diameters of size 30mm and 60 mm. Set the distance between 2 origins at 23mm. Make sure the origin of circles and overall part origin is horizontally aligned (Select two origins while pressing CTRL on keyboard and add horizontal relation).

Go to features tab, select mid plane and using extrude to 60 mm under Direction 1 select Mid Plane as follows.

Clink on a fillet , set radius to 5 mm and highlight the region between two tubes as shown below.

Save the file as Part2.

Part 3: Drawing Bolt

Create a new document from File menu, select Part from Templates and click OK. The units to be used are millimeters.
Select Right Plane, click sketch.
Draw circle of 24 mm diameter.

Go to Features, extrude circle to 8 mm.

Select Chamfer (Expand ), set Distance to 1 mm.

Select the following face and click Sketch.

Draw circle of 16mm diameter.

Go to features, extrude that circle to 105mm.

Select Chamfer, set distance to 1 mm and select lower edge of bolt.

Select Top Plane, click Sketch, draw a circle with diameter of 4mm, set the distance of 84 mm between circle origin and the head.

Go to Features tab, select Extruded cut, choose midplane and cut.

Save the part and name it Part3.

Part 4: Drawing Bolt

Create a new document from File menu, select Part from Templates and click OK. The units to be used are millimeters.
Select Top Plane, click sketch.
Draw 2 circles of size 16 and 24 mm starting from same origin.

Go to Features tab, extrude the sketch to 8 mm.

Select Fillet, set distance to 1 mm and choose outer edge of part.

Select right plane, click sketch and normal to.
Draw a circle with diameter of 4mm above the origin point. Set up 4 mm distance between two origins.

Go to Features tab, using Extruded-Cut cut the hole, under direction1 select Through All-Both.

Save the file as Part 4.

Part 5: Drawing Bolt

Create a new document from File menu, select Part from Templates and click OK. The units to be used are millimeters.
Select Top Plane, click sketch.
Draw 4mm diameter circle,
Go to features tab, select Extruded boss, choose Mid-Plane with distance of 30 mm.

Expand . Select Chamfer, set distance to 0.5mm, select upper and lower edges.

Save the file and name it Part5.

Part 6: Assembly
Create a new document from File menu, select Assembly from Templates and click OK.
Insert Part1 (2 pieces), Part2 (1 piece), Part3 (2 pieces), Part4(2 pieces), Part5( 2 pieces).

Mate (Concentric) the following regions of Part 1 and Part 2.

Mate (Coincident) the following regions of Part 1 and Part 2.

Mate same way another Part1 (first Concentric and then Coincident).

For the convinence purpose we may change the colors of parts by highlighting it and choosing desired color from Edit Appearance tool.

Mate (concentric) the following regions of the parts. Then mate (Coincident) the head of bolt with the face of Part1.

Do the same mating with another bolt.
Now mate (concentric) the following regions.
,
Mate (coincident) the face of bush and face of part1.

By rotating the bush mate (concentric) the wholes of bolt and bush.
Repeat the same process with another bush.
Bring the pin and mate (concentric) with the holes of bush and bolt

Mate (Coincident) the head face of pin and face of bush.

Repeat the process with another Pin.
You have now finished the full assembly of universal joint.