The Charioteers: Wheelchair Lever Arm Design Project

Existing Research and Objective

Market Value Proposition

A way to address upper-extremity weakness in handicapped patients in third world countries that allows them independent transportation is through a socket based lever system which utilizes torque to multiply the force invested into the system by the patient. This lever system will be manifested in a vertical lever with rubberized grips and a housing unit for the sprocket system which offers bi-directional movement in a simple manner. Also, our design allows universally accessible parts that can be repaired or replaced in bicycle stores and mechanic shops around the world.

Current Market

Wheelchairs have been becoming easier to use and cheaper in recent years, with a lot of advancements in engineering having been made starting from the late 19th century. Wheelchairs which are able to function off-road usually sell for $4,500-$6,500, however, some built to target low-socioeconomic-status customers run as low as $200, such as MIT professor Amos Winter’s Leveraged Freedom Wheelchair.

Reference Links:

What Could the Wheelchair Do for the Developing World

CNN Article about Innovative Wheelchairs

Population Needs

The Free Wheelchair Mission has given away wheelchairs to people in 93 countries since 2001. Many of these countries have extremely impoverished areas and rough terrains, both of which should be taken into account. To address the former, we must create an overall product which is cheap which also has cheap, easily replaceable parts. To address the latter, we must create a lever which allows the user to use smaller amounts of force to move greater distances.

Reference Links:

Free Wheelchair Mission

Market Value

Based on cost analysis, this product could be produced for about $65 and sold for $80 with a gross margin of about 25%

Reference Links:

Gross Margin

Small Business Gross Profit Margin

Objective

The wheelchair with a lever arm serves to fulfill the needs of disabled patients on a global scale and allow for independent travel through a low maintenance and low-cost system.

Image Source: A HISTORY OF THE ART OF WAR AMONG THE CARTHAGINIANS AND ROMANS DOWN TO THE BATTLE OF PYDNA, 168 B. C., WITH A DETAILED ACCOUNT OF THE SECOND PUNIC WAR Houghton Mifflin Company, Boston & New York (1891)

Download the McMasterCarr.com parts by clicking on the following hyperlinks and clicking on the save button when the dropdown says "3-D Solidworks". (All parts for the lever arm are given in inches)

For the lever arm part, you will need:

Cushion grips, which you will not need to download as it will be redesigned on Solidworks.

90 degree elbow connectors

Standard-Wall 304/304L Stainless Steel Pipe Nipple, Threaded on Both Ends, 3/4 Pipe Size, 12" Long

Standard-Wall 304/304L Stainless Steel Pipe Nipple, Threaded on One End, 3/4 Pipe Size, 6" Long

The Standard-Wall 304/304L Stainless Steel Pipe Nipple, Threaded on One End, 3/4 Pipe Size, 6" Long is a 6 inch long, threaded on one end pipe. However, this part, which will be the part used by the consumer of the wheelchair lever, needs to be 24 inches long in the design. To fix this, follow the steps below.

Steps:

1) Open the part's downloaded file from McMasterCarr onto your Solidworks program.

2) Click on the plane seen in the picture above.

3) Click on edit sketch, which is in the top left corner as seen above.

4) On the part, it will now be replaced by just a sketch. Find the dimension that says 6 inches and change it to 24 inches.

5) Click on exit sketch

6) Save the part and close the file.

In order to attach the lever arm to the socket mechanism, there needs to be 2 holes created in the double-sided pipe in order to bolt it to the housing of the socket mechanism.

1) Open the double-sided threaded pipe in Solidworks.

2) Click on hole wizard. Choose type to be "hole," the standard to be "ANSI Inch," the size to be 25" and 0.1495in deep, with the end condition as "through all."

3) Close the part.

McMasterCarr does not have any CAD design for the cushioned grips so we need to design a new cushioned grip.

The dimensions are given in the product detail of the part, which will be used in the design of the cushioned grips.

Here are the steps to create your own cushioned grip:

1) Open Solidworks and open a new part.

2) Click on new sketch and click on the button to sketch a circle.

3) Create 2 concentric circles (seen on sketch 2).

4) Click on smart dimension and make the larger circle 0.75 inches in diameter and the smaller circle as 0.245 inches in diameter.

6) Click on boss extrude at the top of the features tab and, in the inputs, make it extrude from the sketch plane, blind, for 6.00 inches. This makes a cylinder 6inches long.

7) Now to make it hollow, click on the inner circle's sketch and, in features, click on extruded cut. Click on from sketch plane and make it cut through all.

8) Exit the sketch.

9) Finally, in the history tree area, click on the materials button and select polyurethane foam flexible to select a material for the grip.

To connect the one-side threaded pipe to a grip, follow the steps:

1) Open a new assembly and insert the new grip part you just built along with the one-side threaded pipe part.

(Click on Mate in the Assembly tab any time the word mate is mentioned.)

2) Mate the inner hollows of the grip and rod with a concentric mate.

3) Create a coincident mate with the edge 1 of the grip and the face 1 (the non-threaded side) of the one-side threaded pipe.

4) Save the file and close it.

Follow the steps to complete the assembly of the lever arm part:

1) Open a new assembly and use insert components to add the grip/one-sided threaded rod, the double-sided threaded rod, and the elbow connector parts.

2) Make a concentric mate with the grips/rod assembly and one of the threaded ends of the elbow connector.

3) Use a screw mate between the thread on the elbow connector and the thread on the one-sided threaded rod with the grip. (Figure 2)

4) Make the last edge of the rod, nearest to the non-threaded part, coincident mated with the face of the elbow connector facing the rod. (Figure 3)

continued...

5) Make the double-sided threaded rod concentric to the empty hole of the elbow connector.

6) Use a screw mate between the thread on the elbow connector and the thread on the double-sided threaded rod with the grip. (Figure 2)

7) Make the last edge of the double-sided rod, nearest to the non-threaded part, coincident mated with the face of the elbow connector facing the rod. (Figure 3)

8) In the end, you will have the completed assembly of the lever arm part, seen in Figure 4.

The engineering drawing of the lever arm is key in manufacturing. Attached is the actual drawing and a video of how I made it. Enjoy!

Please follow this link to watch a video of the lever arm engineering drawing being made.

Roughly sketch out this shape using the line and 3 point arc features, and then fully define this sketch using the dimensions shown in the image above. Then use the extrude boss function to extrude this sketch out by 2 inches.

Create a new sketch on the back face of the handle as shown below, and fully define dimensions and relations according to the picture. Then extrude cut this shape out by 2 inches.

Create a plane using the left and right faces of the handle as your reference points.

Create a rough sketch of the shape seen above, making sure to take note of the radii of the arcs at the top and bottom (Since we are just trying to hollow out a majority of the handle, exact dimensions can vary). Once this has been done, perform a .40 inch extrude cut in the direction of the mid plane.

Create a new sketch on the top back section of the handle, and size a rectangle to the given directions in the picture above. Then extrude cut in both directions, to completely hollow out the top of the brake as shown in the other picture above.

Create a new sketch on the inner front wall of the hollowed out section you just created in the handle, and create a circle that will be extrude cut out 2.81 inches as shown above. Then create another sketch on the same wall, that is rectangular shape dimensioned as shown in the picture above. Then extrude cut this feature 2.81 inches as well.

Create another sketch on either inner face of the handle, making a circle as shown in the figure above (the .25 in measurement is from the center of the circle to the bottom corner of the hollowed out piece of the handle). Then extrude cut out in both directions so that it creates a whole through the whole handle. Then extrude cut another circle on the outer faces of the handle centered on the circle you created just now, but have this circle have a diameter of .30 inches. Extrude cut at a depth of .02 inches. Repeat this on both outer faces of the handle.

Sketch on the outer face of the handle collar, and create a circle of dimensions given in the picture above. Then extrude cut it .34 inches deep. Then sketch on the same plane, making another circle of .30 inches centered at the other circle that you created previously. Then extrude cut it by .02 inches.

Sketch on the frontmost face of the handle, and sketch a circle of the given dimensions in the picture above, and extrude boss outwards .05 inches and .70 inches in the other direction.Sketch on the circular extrusion that you made in the last step, this time creating a circle with a radius of .5 inches, and extrude this out by .15 inches.

Create another sketch on the face of extrusion that you made in the previous step. Create a rough outline of what is shown above, and make sure that the arc has a radius of .08 (this is the most important aspect). Then extrude cut this shape by .015 inches. Then create a pattern for this cut feature, having each one be separated by 60 degrees. You should end up with 6 cuts evenly spaced around the extrusion from step 14.

Create another extrusion on the face of the same extrusion that you have been working on, this time making a circle in the center that is .2 inches in diameter. Then extrude outward by .05 inches. Create a new sketch on the plane made in step 3, making the rough shape shown in the figure below. Then dimension out everything according to the image. Then revolve the shape around for 360 degrees.

Sketch on the back face of the revolve feature, and make the basic shape shown in the diagram above (Make sure the radius is .08 inches). Then extrude cut by .39 inches. Then create a circular pattern and make sure they are separated by 60 degrees for a total of 6 cuts total.

Use the convert entities feature to convert the inner face of the handle, and then add a line roughly where it is shown in the diagram below, and trim the top portions. Once only the shaded yellow portion of the figure above is sketched, extrude it out .10 inches. Then mirror the extrusion you just made across the plane from step 4 as shown above.

This part is now complete, and is ready to be put in an assembly later on.

Create a new part, and sketch on the front plane this shape, with the dimensions seen in the picture above. Then, extrude this part out by .20 inches. After this, use the convert entities feature on the face, and trim the bottom part so that only the highlighted part in the image above is left. Then extrude it out by .05 inches. Repeat this on the opposite face.

Make another sketch on the same face, creating a rough sketch of what is shown in the image below. Use the spline feature for this and, while it does not have to be exact, it should have a pretty similar shape. Then extrude the shape through all.

This part is now done and ready to be placed in an assembly later on.

Create a new part, and sketch and dimension according to the image above. Then revolve this sketch by 360 degrees and this part is finished as well.

This part is now done and ready to be placed in multiple assemblies.

Create a new assembly, and then add all 3 parts. Make the hole at the bottom of the lever concentric to the hole at the bottom of the hollowed portion as shown above.

Use a width mate with the width selections as the two inner faces of the handle, and the tab selections as the faces of the lever as shown above.

Make the hole at the bottom of the hollowed part of the handle concentric to the bottom edge of the pin, and then make the bottom face of the pin coincident to the hole on the outer part of the handle so it sits flush. Insert another pin and repeat this process on the other side of the handle. The tolerance for this fit is a ±.05 inches.

This assembly is now complete and ready to be used.

1.) Create a new engineering drawing and use the A3 (ISO) format.

2.) Import the proper brake assembly file, and add 2 different model views, a standard three view and an isometric one. This should come out to 4 different views total You can also adjust for these to show hidden lines in the options for each of these views at any time. 3.) Smart dimension out any relevant measurements, and make sure that all drawings are scaled appopriately as well (in this case, a 1:2 scale worked fine) 5.) Fill out the table at the bottom right by editing sheet format under the sheet format tab. From here, you can write the name of the company, the project and part being depicted, as well as who designed it and when, and etc. Be sure to adjust font as need be so that it is readable, and do that for any notes or balloons you may have as well. Also, remove any unnecessary lines or boxes in the table using the trim sketch feature.

1) Use the IPS unit system.

2) Create a sketch of a circle with a diameter of 0.15 in

3) Use the “Extrude Boss” feature to extrude the circle to a length of 30.0 in

The brake caliper will be an assembly separated by 3 major parts: One half of the caliper, another half of the caliper, and the pin in the middle which connect the caliper halves together and attach the caliper assembly to the actual wheelchair assembly. The first half of the caliper will reflect the image below.

1) The first step in this part is to create a sketch using the IPS unit system.

2) Start off the sketch at the origin of the front plane by drawing vertical and horizontal centerlines upwards and to the left of the sketch. Then draw another centerline to the left of the vertical centerline, starting at the horizontal line and drawing upwards. Smart dimension this centerline to be 2.90 in away from the vertical centerline which starts at the origin.

3) Create an arc, with the radius exactly 1.41 in above the origin. Draw another arc with radius 1.93 in. The radius for both arcs should lie on the vertical centerline. Then draw another arc to connect the top of the two arcs, but this arc should have a radius of 0.26 in and it should start and end at points on the centerline. Draw 2 smaller circle in the at the radius of this small arc of radii 0.16 in and 0.28 in. *See picture for reference

4) Create a small sweep started at the outside arc and going to the left, then draw another sweep under that arc. Then draw two horizontal lines of length 1.17 in from the ends of both sweeps. Draw a small arc connecting the two horizontal end segments. Draw a vertical centerline from the radius of that arc. Smart dimension the distance between this centerline and the vertical centerline at the origin to be 2.90 in.

5) At the bottom of the two large arcs, draw two vertical lines from the endpoint and connect them both with a 0.50 in horizontal line.

6) Extrude the entire shape by 0.20 in.

7) Turn the shape to the Right plane and click on the bottom vertical plane, Then draw a rectangle of width 1.5 in and length 0.7 in and extrude this shape by 0.25 in.

Start a new part in SolidWorks for the other half of the brake caliper. ** See pictures for reference on how to build parts

1) Create two large arcs with radii 1.41in and 1.93in. These should be about ¾ of the circumference of a circle. On the right, repeat the vertical lines from the bottom of both arcs and connect them with a horizontal line of 0.5 in. On the right side, create a small sweep and extend a small gap for a cylinder with radius 0.20 in.

2) At the bottom of the two large arcs, draw two vertical lines from the endpoint and connect them both with a 0.50 in horizontal line.

3) Extrude the entire shape by 0.20 in

4) Create a hole that extends through the cylinder and thru the horizontal gap of the first caliper half. This hole should have a radius of 0.08 in and should vertically align for both parts.

5) At the center of the large arc in the middle, create two concentric circles with radii 0.16 in and 0.28in.

6) To mate these two parts, Concentric and coincident mate the holes from the step above of both of the parts.

1.) Create a new engineering drawing and use the A3 (ISO) format.

2.) Import the proper brake assembly file, and add 2 different model views, a standard three view and an isometric one. This should come out to 4 different views total You can also adjust for these to show hidden lines in the options for each of these views at any time.

3.) Smart dimension out any relevant measurements, and make sure that all drawings are scaled appopriately as well (in this case, a 1:2 scale worked fine)

5.) Fill out the table at the bottom right by editing sheet format under the sheet format tab. From here, you can write the name of the company, the project and part being depicted, as well as who designed it and when, and etc. Be sure to adjust font as need be so that it is readable, and do that for any notes or balloons you may have as well. Also, remove any unnecessary lines or boxes in the table using the trim sketch feature.

1) Use the IPS unit system

2) Import the Brake Handle, Brake Wire, and Brake Caliper to the assembly.

3) Coincident mate one tip of the wipe to the flat 0.15 in circle in the brake lever. *See picture for reference

4) Concentric Mate the wire through both the holes of the caliper. These holes are vertically aligned so the wire should fit through perfectly.

5) Lastly, coincident mate the other end of the wire to the flat bottom of the cylindrical barrel to make the wire end flat at the caliper.

1.) Create a new engineering drawing and use the A3 (ISO) format.

2.) Import the proper brake assembly file, and add 2 different model views, a front view and an isometric one. You can also adjust for these to show hidden lines in the options for each of these views at any time.

3.) Smart dimension the length of the wire, and add balloons to the front view by using the feature under the annotation tab (you can also add notes to show which view is which as well).

4.) Create a bill of materials by going to insert, then table, and bill of materials. If you have already determined the materials for each part, and added materials to the table you should be fine. Otherwise go to each individual part and assign it a material.

5.) Fill out the table at the bottom right by editing sheet format under the sheet format tab. From here, you can write the name of the company, the project and part being depicted, as well as who designed it and when, and etc. Be sure to adjust font as need be so that it is readable, and do that for any notes or balloons you may have as well. Also, remove any unnecessary lines or boxes in the table using the trim sketch feature.

• Boss-Extrude2
  • Create a sketch on the front plane.
  • Sketch an 11 mm circle (1 mm clearance for the shaft) with the center at the origin. Sketch another circle concentric to the 11 mm circle. Smart dimension the diameter of the second to 30 mm.
  • Create a vertical centerline that bisects the two circles along the origin.
  • Sketch a rectangle with its bottom corners coincident with the arc of the 30 mm circle. Using trim entities, deleted the bottom edge of the rectangle. Use a tangent arc to create the curved teeth of the gear; the points of the tangent arc should be coincident with the top corners of the rectangle. Using trim entities, delete the top edge of the rectangle.
  • Create an equal length relation between the remaining left and right edges of the rectangle. Also create a symmetric relation between those sides along the vertical centerline.
  • Smart dimension the radius of the arc to 2 mm and the length of the sides to 8 mm. Set the angle between the sides to 30 degrees.
  • Create a circular sketch pattern of the arc and the two sides around the 30 mm circle. Make a total of 10 teeth.
  • To make sure that the sketch is fully defined, create coincident relations between the end points of each patterned tooth to the 30 mm.
  • Extrude the space of each tooth and the space between the 11 mm circle and the 30 mm circle to 10 mm.

• Fillet 3
  • Fillet the arc between the ends of the teeth with a symmetric fillet to a 1.00 mm radius. The profile should be set to Conic Rho with rho set to 0.5.

• #27 (0.144) Diameter Hole1
  • Since you need close fit holes for 6-32 hex bolts, you have to use a #27 drill size to create the holes on the gear using Hole Wizard.
  • Set the hole type to Hole and the standard to ANSI Inch. The hole size is #27.
  • To set the position of the holes, create a sketch through the Positions tab on hold wizard.
  • Create vertical and horizontal centerlines that intersect at the origin. Create two diagonal centerlines that cross at the origin and use smart dimension to set their angle relative to the horizontal line to 45 degrees.
  • Place a hole on each line created by the center lines (there are 8) and set their position along the centerline to 12 mm away from the origin. Exit hole wizard with the green check mark.

• Boss-Extrude1
  • Create a sketch on the Front Plane.
  • Sketch a rectangle starting at the origin. Smart dimension the length of the rectangle to 40mm and the width to 6mm.
  • Sketch a circle inside the rectangle, towards the top. Make tangent relations between the arc of the circle and the top, left, and right lines of the rectangle. This sets the diameter of the circle to 6mm.
  • Sketch an angle line from the corner of the rectangle at the origin to the opposite line. Set the angle between the line at the origin and the angled line to 38 degrees. Trim the bottom right corner to create an angle.
  • Extrude Boss/Base the sketch containing only the circle and the region of the original rectangle under the circle and above the angled line to 12mm.

• #25 (0.1495) Diameter Hole1
  • Since you need a free fit hole for a 6-32 hex bolt, you have to use a #25 drill size to create the holes on the gear using Hole Wizard.
  • Set the hole type to Hole and the standard to ANSI Inch. The hole size is #25.
  • To set the position of the holes, hover over the half-circle arc to find its centerpoint. Set the centerpoint of the hole to the same centerpoint of the arc to make the hole concentric to the arc.

• Fillet1
  • At the corner of the rectangle at the origin, create a fillet with a radius of 1mm.

• Sweep1
  • Create a sketch on the Top Plane. Make a horizontal centerline and a vertical centerline with the corner at the origin. Set the length of the horizontal centerline to 0.20 inches using smart dimension.
  • Create another sketch on the top plane. Sketch a circle with its center at the end of the horizontal centerline and set its diameter to 0.035 inches.
  • Create a swept boss/base and select sketch profile. Select the sketch of the circle for the Profile and the sketch of the horizontal and vertical centerlines for the Path.

• Revolve1
  • Create a sketch on one of the ends of Sweep1 (the flat circular face). At the center of the face draw a vertical center line towards the inside of the sweep.
  • Sketch a horizontal normal line from the edge of the circle to its centerpoint.
  • Sketch a centerpoint arc with the center at the center of the circular face. The first point of the arc is coincident with the edge of the circular face and the horizontal normal line. The second point of the arc is coincident with the edge of the circular face and the vertical centerline.
  • Use revolve boss/base with the vertical centerline as the axis of revolution and the connected line and arc sketch as the contour to revolve. Revolve to 180 degrees.

• Revolve3
  • Repeat the steps from Revolve1 except with the other end of Sweep1 (the other flat circular face).

• Sweep5
  • Create a sketch on the remaining face of the circular end. Sketch a line from the center and make it vertical using add relations. Smart dimension the line to 0.25 inches.
  • Sketch another line with its first point coincident to the end of the 0.25 inches line. Make is horizontal using add relations. Smart dimension the line to 0.25 inches.
  • Using sketch fillet, select the vertical and horizontal lines and set the radius to 0.05 inches.
  • Create a circular profile sweep and use the sketch made in the previous step as the Path. Set the diameter of the sweep to 0.035 in.

• Sweep2
  • Repeat the steps from Sweep5 except with the other end of Sweep1.

• Boss-Extrude1
  • Create a sketch on the top plane. Sketch a vertical line that goes through the origin. Smart dimension the vertical line to 8 mm.
  • Use a centerpoint arc at the top point of the vertical line and smart dimension the arc to a radius of 4 mm.
  • At the other end of the vertical line, create another centerpoint arc with a radius of 14 mm.
  • Connect the arcs with lines. Make the left endpoints symmetric to the right endpoints along the vertical line.
  • Extrude the sketch to 7.62 mm.

• Fillet1
  • Fillet the left line and the arc with a 14 mm radius and fillet the right line and the arc with a 14 mm radius.
  • Set the radius of the fillet to 5.00 mm with a symmetric, circular profile.

• Boss-Extrude3
  • Sketch a circle 6 mm in diameter that is concentric to the 4 mm radius arc from Boss-Extrude1.
  • Extrude boss/base the circle to 4.38125 mm.

• Boss-Extrude5
  • Sketch a circle concentric and equal in diameter to the 4mm radius arc from Boss-Extrude1.
  • Extrude boss/base the circle to 2.00 mm.

• #25 (0.1495) Diameter Hole1
  • Since you need a free fit hole for a 6-32 hex bolt, you have to use a #25 drill size to create the holes on the cam lock using Hole Wizard.
  • Set the hole type to Hole and the standard to ANSI Inch. The hole size is #25.
  • To set the position of the holes, hover over the circle extrusion to find its centerpoint. Set the centerpoint coincident to that centerpoint.

• Cut-Extrude2
  • The sketch (which is related to the cam switch) will be created in the ratchet mechanism assembly.

• Boss-Extrude1
  • Create a sketch on the top plane. Sketch a vertical centerline along the origin.
  • Sketch two concentric circles and use smart dimension one to 3.50 mm and the other to 6 mm.
  • Sketch four vertical lines on the inside of the circles. Two should be to the left of the vertical centerline and two should be to the right of the vertical centerline. Add a collinear relation between the lines on the left side and between the lines on the right side. Add a parallel relation and a symmetric relation between the lines that are on opposite sides of the vertical centerline.
  • Smart dimension the distance between the lines to 3.00 mm.
  • Use trim entities to remove the arcs of the circles not within the 3.00 mm region.
  • Extrude the regions to 2.38125 mm.

• Boss-Extrude2
  • Create a sketch on the bottom face of Boss-Extrude1. Sketch circles concentric and equal in diameter to the arcs in Boss-Extrude1.
  • Extrude the region between the circles to 2.38125 mm.

• Boss-Extrude3
  • Create a sketch on the bottom face of Boss-Extrude2. Sketch a rectangle with the top edge collinear with the horizontal centerline and the corners coincident with the arc of the circles in Boss-Extrude1.
  • Add symmetric relations to the left and right edge of the rectangle along the vertical centerline of Boss-Extrude1. Smart dimension the length of the rectangle to 25 mm.
  • Sketch a circle with a diameter of 3.5052 mm. Sketch a concentric arc with its endpoints coincident to the top corners of the rectangle. The arc has a diameter of 8 mm.
  • Use trim entities to remove the top edge of the rectangle.
  • Extrude boss/base the sketch to 5.00 mm.

• Go to mcmaster.com and search for the steel shaft with the product number “1482K110”. Download the Solidworks .sldprt file for it.
• Adjust the length of the shaft by editing Extrude1 and changing the mid-plane extrusion length to 40 mm.
• To make the grooves for the retaining rings, select the right plane and create a sketch.Sketch two rectangles with their top sides collinear with the cylindrical face of the shaft. Set the width of the groove to 1.1 mm using smart dimension. To set the groove depth, set the length to 0.2 mm using smart dimension.
• Use revolved cut around the center axis of the shaft to create the grooves out of the two rectangles. The position of the grooves will be set later in assembly.

• Boss-Extrude1
  • Create a sketch on the Top Plane. Sketch a circle with the center at the origin. Smart dimension the diameter to 127 mm. Extrude boss/base the sketch to 4.7625 inches.

• Boss-Extrude2
  • Create a new sketch on the top face of the extrusion in the previous step. Sketch a circle concentric and equal to the extrusion in the previous step. Sketch another concentric circle. Set the distance between the circles to 6.35 mm using smart dimension. Extrude the region between the two circles to 15.00 mm.

• Cut-Extrude1
  • Create a sketch on the top face of the extrusion and sketch a circle with a diameter of 10.01524 mm. (The shaft is 10mm in diameter, thus the hole needs a 0.01524mm tolerance for a class RC 3 fit.)
  • Extrude cut the sketch through all.

• Cut-Extrude2
  • Create a sketch on the top face of the extrusion and sketch a horizontal centerline that goes through the origin. Sketch a vertical line on both sides of the center shaft hole.
  • Sketch a circle at each intersection of the centerlines and smart dimension the circle to 0.1495 in (provides a free fit for 6-32 hex bolts).
  • Smart dimension the distance between each circle and the origin to 38.10 mm.
  • Extrude cut the sketch through all.

• Cut-Extrude3
  • The holes (which are for the pawls and the cam switch) are based on a sketch in the ratchet mechanism assembly

• Cut-Extrude4 and Cut-Extrude5
  • The holes (for the springs) are based on sketches in the ratchet mechanism assembly.

• Boss-Extrude1
  • Create a sketch on the Top Plane. Sketch a circle with the center on the origin. Smart dimension the circle to 5.50 inches. Extrude boss/base the circle to 0.25 inches.

• Boss-Extrude2
  • Create a sketch on the top face of the extrusion made in the previous step. Sketch a circle that is concentric and the same diameter as the circle in the previous sketch. Sketch another concentric circle and set the distance between the circles to 0.25 inches. Extrude the region between the circles to 0.25 inches.

• Cut-Extrude1
  • Create a sketch on the top face of the extrusion and sketch a circle with a diameter of 10.01524 mm. (The shaft is 10mm in diameter, thus the hole needs a 0.01524mm tolerance for a class RC 3 fit.)
  • Extrude cut the sketch through all.

• #27 (0.144) Diameter Hole1
  • This is created within the ratchet mechanism assembly according to the holes on the sprocket gear.

• Go to mcmaster.com and search for the retaining rings with the product number “90967A160”. Download the Solidworks .sldprt file for it.

• Go to mcmaster.com and search for the 6-32 hex bolts with the product number “93075A546”. Download the Solidworks .sldprt file for it.
• Go to mcmaster.com and search for the 6-32 hex nuts with the product number “90631A007”. Download the Solidworks .sldprt file for it.

• Create an assembly. Insert the shaft as the first component (it will be the fixed component).
• Insert the housing lid, make its center hole concentric with the shaft, and make the inner circular face face the middle of the shaft. Mate its outer face 8 mm away from an end face of the shaft.
• Insert the sprocket gear, make its center hole concentric to the housing lid, and make one of its faces coincident with the inner circular face of the housing lid.
• Edit the housing lid and make eight #27 holes using hole wizard that are concentric to the holes on the sprocket gear.
• Insert the housing into the assembly, make its center hole concentric with the shaft, and make the top face of its lip concentric to the inner circular surface of the housing lid.
• On the top plane, create a sketch with the given dimensions in the image above. The bottom point of the vertical centerline should be coincident with the center of the shaft.
• Mate the inner circular face of the housing coincident to the assembly’s sketch.
• Insert the cam lock and the cam switch. Make the holes for the hex bolts concentric to each other. Make the cam lock’s hole concentric to the middle hole on the sketch. Mate the side face of the extrusion on the cam switch coincident with the cut extrude on the cam lock such that the switch’s length is facing the opposite direction of the lock’s longer arc. Mate the face of the cam switch right under the extrusion coincident to the outer face of the housing lid. Insert two pawls and orient them such that the angled face faces outward of the housing. Make one pawl’s hole concentric to the left hole on the sketch. Make the other pawl’s hole concentric to the right hole on the sketch.
• Edit the housing. Using convert entities, add the holes from the pawls and the cam lock/switch to the housing. Extrude cut through all.
• Insert two springs into the assembly. Mate their center axes 0.25 inches away from the inner circular face of the housing. Make a plane normal to the center axis and coincident to the end of the coil with the longer grip extrusion and mate it 1.375 inches to the center point of the sketch where the vertical centerline and angled centerlines intersect. Mate the center axis of the spring coincident to a plane that goes through the angled centerline. Do this for both springs.
• Insert the retaining rings and make them concentric to the shaft. Mate the top face of the retaining ring coincident with a side face of a groove of a shaft. Repeat with the other retaining ring except with the opposite groove.
• Edit the shaft and make the inner side face of one of the grooves coincident with the outer face of the housing lid. Do the same with the other groove, except make it coincident with the outer face of the housing.
• Add hex bolts and nuts using concentric mates for the hole extrusions, coincident mates, and mechanism screw mates to the holes on the pawls, cam lock/switch, and the sprocket gear. The cap of the hex bolts should be inside the mechanism while the hex nuts should be on the outside faces of the mechanism.

• Housing Lid with the sprocket gear

• Housing with the ratchet mechanism

• Insert the lever arm assembly into a new assembly. It will be the fixed component.
• Insert the ratchet mechanism assembly.
• Edit the shorter steel pipe within the assembly.
  
  • Create a reference axis that goes through the length of the pipe.
  • Using hole wizard, make #25 drill size holes on the front plane that extrude through all. Smart dimension one hole 1.5 inches away from the open end of the pipe.
• Make a parallel mate between the reference axis of the shorter pipe to the vertical centerline on the housing of the ratchet mechanism.
• Make a concentric mate with the left hole on the housing of the ratchet mechanism to the left hole on the pipe.
• Make a tangent mate between the cylindrical face of the pipe to the outside face of the ratchet’s housing.
• Edit the short steel pipe and make a relation between the second hole on the pipe to the second hole on the ratchet mechanism’s housing.
• Add in the 6-32 hex bolts and nuts using screw mates, concentric mates, and coincident mates such that the cap of the hex bolts are inside the ratchet mechanism and the hex nuts are on the outside of the steel pipe.

1) Standard-Wall Unthreaded PVC Pipe for Water, 3/4 Pipe Size, 5 Feet Long is the link to the PVC pipe used to make the lever arm. We ordered 2 of these pipes, along with 2 elbow connectors for the purpose of creating a 90 degree angled lever arm that will not interfere with the ratchet mechanism.

2) For each PVC pipe, a 24" section and a 12" section was cut using PVC pipe cutters to make 2 pipes that can be connected with the elbow connector into a 90 degree angle.

3) A drill was used to make 0.138" diameter holes in the shorter PVC section according to where it would attach to the housing unit of the ratchet mechanism.

4) A larger hole was also drilled to create a 100mm diameter hole for the metal shaft in the housing.

5) A piece of wood was cut to insert in the cushioned grip to create a proper handle for the brake handle to attach to. Duct tape was used to connect the brake handle to the grip, as the wrong parts had been shipped and wouldn't fit as snuggly as expected.

6) The housing was then attached to the lever's shorter end using bolts and a retaining ring with the shaft, which will be explained later.

Please see the picture above for proper visuals!

1) Order 2 sets of side-pull caliper bike brakes

a. The Set we ordered was the: Sunlite Side Pull Brake Set, 61 - 79mm Reach, Silver (See hyperlink for reference)

2) Unscrew the nut on the right of the caliper and expose the push holes for the brake wire to go thru. Pull the wire through the top hollow screw and the pin holes in the caliper screw, then tighten the nut to prevent movement.

3) Slide the wire into the brake lever and slide the locking mechanism into place

4) To assemble on the lever arm, slide a textured grip into the hole at the top of the PVC pipe acting as the lever arm. Place the brake around that grip.

5) To place the caliper on the wheels, get a ¾ in PVC pipe of length ~4in and drill 3 holes vertically spaces 1 in apart from each and from the edges. Make sure the the holes drilled are large enough to fit the long screw at the middle junction of the caliper. Then slide the screw into a hole that fits the height (the middle hole) and tighten the nut to ensure it doesn't slide out.

6) Place the caliper onto the wheel and then tighten the caliper so that it will effectively brake

7) Hold the PVC pipe horizontally (perpendicular to the wheel) next to the back support of the wheelchair. Zip tie the hole in the PVC pipe to the side rails of the wheelchair that run parallel to your back when sitting.

8) Test the brake to ensure that it works properly

3D Printed custom parts (Refer to solidworks files for parts sizing)

• Sprocket
• Pawls
• Cam lock & Switch

Off the shelf parts (Refer to manufacturing instructables for off the shelf sizes/specifications not provided below)

• Hexbolts
• Shaft
• Lock nuts
• Wooden pieces for support (Use scrap wood and cut to size)
• Retaining Ring
• Circular wooden box for the housing compartment (10 in in diameter)

Additional Tools:

• Drill with various drill bits
• PVC Cement Glue
• Ruler
• Pliers

1. Drill the holes displayed in the image. The center hole will provide space for the shaft and the remaining holes will allow the pawls, cam lock, and lever to be fastened.
   This includes:
   • A 10mm diameter hole in the center to pull the shaft through
   • A 3.51 mm diameter hole approximately 37.21 mm to the right of the housing center. This will be used to attach the lever arm with hex bolts
   • A 5mm diameter hole 44.17mm above the housing center
   • A 3.51 mm diameter hole to the right and left of the hole drill in the previous step
2. Assemble the inner components of the main housing unit. Use heavy duty PVC cement glue to attach several inner components:
   • The springs onto a supporting piece of wood
   • The top of the spring to the pawl
   • The supporting wood piece into the main housing uni
3. Ensure that the position allows the pawls to engage with the sprocket.
4. Fasten the cam lock in between the pawls

1. Drill a center hole 10mm in diameter for the shaft.
2. Drill 8 equidistant 2.79 diameter holes 5.78mm away from the edge of the center hole
3. Attach the sprocket to the lid using hex bolts. Secure the underside with lock nuts.
4. Create a slot to move each slot. This will give the user control of the direction they're moving in.
   • Mark the spacing between the camlock and the pawl.
   • Move the pawl toward the spring until it is completely compressed.
   • Mark the pawl's path and cut a slit big enough to fit a hex bolt.
   • Cut the slit vertically up to create a lock position for the slot.

1. Close the main housing unit and the lid. Add the shaft through the middle and insert the retaining rings on each side to hold everything together
2. The Assembly should allow the pawls to engage with the sprocket. Move one of the pawls out of the way and rotate the lid with respect to the housing unit. Ensure that the pawls make a clicking sound when pushed back. The pawls should get caught in the opposite direction.
3. Attach the lever to the main housing unit
4. Attach the final prototype to the wheel using zip ties in between the spokes.
5. The prototype is complete!

Design Constraints:

The lever itself is a crucial component of the wheelchair. It is the part that connects the user to all the mechanical parts moving the chair. The main design constraints to worry about with this part the material stiffness, weight, and the cost, as well as comfort of the arm position. The lever must be lightweight to allow a user with upper-extremity weakness to move the arm with minimal force. The lever must also be strong to minimize the possibility of the material bending or undergoing deformation while force is being applied. Lastly, because this lever arm is being designed for third world countries, the material must be resistant to corrosion to maximize the length of time it could be used before being replaced.

Design Objectives:

1. Minimize weight
2. Maximize mechanical strength
3. Maximize Resistance to corrosion

Material Chosen: Stainless Steel

Stainless steel is a good choice for the lever arm because it is easily machinable, very strong, and resistant to corrosion. With a modulus of elasticity of 193-200 GPa and a yield strength of 550 Mpa, steel provides a high strength material that could withstand the force applied while the lever arm is in use. This material is also highly resistant to corrosion, allowing the user to get more use out of the product because having to purchase a new one.

Design Constraints

The brake allows the user to stop the chair when needed by using a brake pad to apply sufficient friction and stop the motion, often generating substantial heat. The brake material must be able to withstand this heat buildup while also limiting the cost of the material. The brake pads must also be rough enough to apply the appropriate friction needed to stop the chair’s motion.

Objective

Maximize tear resistance
Maximize tensile modulus

Materials Chosen:Rubber

The nature of the brake implies that the brake will undergo constant tensions as it constantly rubs against other materials. Rubber has a tensile strength of 10-25 MPa, making it resistive to strain even under significant stress. Additionally, rubber’s high tear strength ensures that the material will not develop slits or cuts when tension is applied.

The socket Wrench Mechanism moves the entire wheelchair, making it one of the most important parts of the final product. The main concern for this system was to ensure that the material of each part was strong enough to allow the pawls to move the weight of both the wheel chair and the weight of an individual.

Design Objectives:
Optimize Strength
Minimize weight

Material Chosen: Aluminum 2024-T861

Aluminium 2024 Alloy has a high strength-to-weight ratio, making it the best material for the socket wrench mechanism. It has a yield strength of 500 MPa. This material’s strength ensures that the mechanism is capable of moving the wheel, even when the load of an individual is added. The light weight material also reduces the amount of force the individual has to apply to move the entire mechanism. Lastly, using aluminum makes the part easily accessible and therefore easily replaceable, if needed.

During the iterative testing process, we fixed a few problem of the original prototype’s problems. An example of this is that the first set of springs had too high of a compression rate so we had to swap out the original springs we had for a weaker set of springs so that the pawls and gear could function properly. This change allowed the mechanism to move smoothly. Another change that occurred during testing occurred to the cam switch mechanism. This was supposed to move the pawls so that the user could switch between forwards and backwards. This switch mechanism broke during testing so we built a slot in our housing unit and used a hex bolt to switch between going forwards and backwards. A last change we made was adding supports inside of the housing unit to create a stronger device that could handle more force given the materials the prototype is made out of.

Our lever is easier to use than the push rim because by increasing the distance from the center of the wheel, less force needs to be applied by the user to have the same work output. Based on measurements, the user needs to exert about 39% of the force they would use on the push rim to result in the same amount of work. Furthermore, this means that if the user applied the same amount of force to the lever as they would have to the push rim, the resulting work would be more than double the amount resulting from the push rim alone. This shows that our lever has a clear mechanical advantage over the push rim.

The equation for torque is similar to the equation for work (replace work with torque and replace distance with radius). The biggest difference between the two is that torque takes angle into account. However, if we are using measurements found with the same angle, this angle is negligible for comparison. Therefore, torque has the same mechanical advantage with our lever, resulting in 39% of the force applied to the push rim creating the same amount of torque.

Using equations for work and force, it is demonstrated in the picture that work is directly related to velocity. As it was proved in the previous sections that less work will be needed with the lever for the same output, similarly, less work is needed to create the same velocity. Since work and velocity are directly proportional, if 39% of the work applied to the push rim were to be applied to the lever, the velocity output would be the same. This ultimately means that if the user were to use the same amount of force they used on the push rim, they would be able to go considerably faster (once again, more than two times the previous amount) than they were able to without the lever.

A spreadsheet was created to list the materials used to build the prototype as well as the cost for each.

Total cost: $111.42

The prototype attempted to model the manufactured product with a few minor substitutions. The materials for the prototype are listed on the spreadsheet.

A spreadsheet was created to list the items used and the total cost.

The total cost for the manufactured lever arm is $65.36.

Keeping the target audience in mind, our group was careful to ensure that the lever arm was cost-efficient. The final product is well under $70, making it accessible to populations in third world countries regardless of socioeconomic status.