The common wheelchair contains many flaws for those with upper extremity weakness or limited resources. Our team was tasked to design a wheelchair lever driver for the wheelchairs from the Free Wheelchair Mission that would allow users to go farther in their chairs and help those with upper extremity weakness use the chairs. The Support System wheelchair lever driver is a cost-effective device that substantially lowers the need for shoulder motion and addresses fatigue levels by utilizing horizontal lever drivers rather than vertical, which would be suitable for weakened patients and patients in rural areas. The typical vertical lever arm driver focuses too much on the muscles in the arms and shoulders, which can cause complications for patients with upper extremity weaknesses. Therefore, our team designed a horizontal lever driver that aimed for usage of the chest muscles to bring ease for people who cannot utilize their shoulder muscles.
Market and Value Proposition
A way to address the shoulder pain and fatigue that is associated with wheelchair usage in individuals particularly from rural villages with non-paved roads, our lever driver aims to alleviate the problem by using forward/ backward motion rather than an up/down motion along with an improved armrest for comfort and support. Because rural villages and non-paved roads are commonly very rocky and unsmooth, the patient would have to use even more force to the lever arm in order to move their wheelchair to a certain distance in comparison to a smooth path. Therefore, the people with upper extremity weaknesses in rural areas are even more hindered because they require more movement and strength to move place to place, which causes problems as they continuously grow weaker as they continue to utilize their shoulder muscles on a day to day basis. Thus, by implementing a horizontal lever driver, individuals from rural areas with upper extremity weaknesses will not only be able to move freely but also in a way that reduces the strenuous use of the shoulder muscles as they use the strength in their chest instead.
We decided to use PVC, acrylic, and ABS. It was a compromise of strength and cost. The three materials are relatively cheaper, but sturdy enough to function properly. The estimated cost is about $170. We originally planned on using aluminum for most of the components of our lever driver such as the outer case and the arm handles because aluminum is cheaper than steel. However, after doing research, we saw that using thick sheets and rods of aluminum would not be ideal because of the outstanding costs to obtain substantial amounts of metal. Instead, we found cheaper alternatives by using different materials for different parts. We used a large acrylic sheet for the outer casing and laser cut the sheet into smaller parts, which came out to about $25. In comparison, large aluminum sheets would have cost over $70. In addition, we also decided to use PVC pipes for our arm handles instead of metal rods because PVC pipes are not only sturdy, but also extremely cheap as well. Although aluminum rods may have been sturdier, we would have spent around $30 on each side of the wheelchair. In contrast, the PVC pipes came out to around $5 in cost. The bulk of our cost comes from the ABS 3D printing. Because we printed three parts of our system, the total time to print all these parts took a total of around 32 hours. As a result, with the hourly rate to use the 3D printer, the total came out to $130.
Materials and Prototyping Design
- PVC pipe ~ $2.16
- PVC socket cap ~ $1.66
- PVC 90-degree elbow ~ $2.28
- Acrylic sheet ~ $24.98
- ABS gears, ABS pawls, ABS knobs ~ $130
- Steel screws ~ $6.92
- Rubber bands ~ $3.18
- E6000 Craft Adhesive ~ $4.29
Step 1: Create the Outer Casing Lid for the Body on SolidWorks
Before starting the entire project, set the dimensions using MMGS.
Using the front plane, create a new sketch and draw a circle at the origin with a diameter of 175mm. Then, sketch two vertical lines at the tangents of the circle that are both 60mm. After, draw tangent arcs at the end of both lines and connect them with a horizontal line. Then using the feature "trim entities", trim the lower half of the circle inside the region.
Once the sketch is completed, boss extrude the sketch using a blind extrusion by 12.70mm. Once the extrusion is complete, open up a new sketch and draw a circle lining up with the top of the tangent lines with the diameter of 32.20mm and cut extrude using "through all" make a hole.
To make the bottom two circles, open a new sketch and draw two circles with the diameter of 6mm and make them 15mm away from the bottom and 58.84mm away from the center of the tangent arc. Once the sketch is complete, use cut extrude using "through all" to make two holes.
Step 2: Create the Body on SolidWorks
To start the body, repeat the sketch as in part one to create the overall shape of the body and extrude it 25.40mm. After the part is extruded, use the shell option on one of the faces of the part with the dimension 12.70mm.
After, open a new sketch and draw a circle at the center of the part with the diameter of 100mm that is 133.84mm from the bottom and 87.50mm away from the sides of the part. Once the sketch is complete, cut extrude using "through all" once again to create a hole.
To create the lever, create a new sketch on the top plane and rotate the part to the bottom. Start off the sketch by making a circle with a diameter of 28.74mm at the base of the previous part and extrude it 130mm.
Once the lever is created, create a new sketch at the base of the lever. Draw two horizontal lines equidistant from the origin that is 25.10mm long. After, connect the two lines with tangent arcs with the height of 14mm. Once the sketch is complete, blind extrude the new sketch 30mm.
Using the newest extruded part, create a new sketch on the front plane and sketch a circle that is 14.95mm away from the top and 12.55mm away from the side. Then, cut extrude through all to create a hole.
With the overall body, sketch two holes at the bottom of the body with diameters 6mm and distance 36mm away from each other, 15mm away from the bottom, and 58.84mm away from the top of the tangent arcs. After, cut extrude through all to create two holes.
On the bottom of the part, create a new sketch. Make straight lines on both sides that are 14.93mm. Make a horizontal line that is 28.74mm to connect the two lines. Draw a circle that has a 14.37mm radius and align it to the circle in the center already. Trim it to make a half circle. Cut extrude through all the ramp-shaped figure in the bottom of the part to leave a rounded edge.
*To prepare for the cavity, create a new sketch in the back plane. Draw a circle with a 20.57mm radius 15mm away from the bottom, and 58.84 from the side tangent arc. After assembling all the pieces together, you edit the part within the assembly and use the cavity feature to create the semi circles.
On the front plane, make a new sketch. Draw a circle in the center with a 6.35mm diameter between the big circle and the two small circles near the bottom. Make the circle 40.13mm away from the bottom and 33.70mm away from the tangent arc on the sides. After, cut extrude through all to create a small circle in the center.
*This step is to be continued on later after assembling all the pieces together.
Step 3: Create the Joint on SolidWorks
To begin the join, start by creating a new sketch on the front plate and draw a circle with the diameter of 28.74mm. Blind extrude the circle that was just sketched 120mm.
Then, rotate the part and sketch on the back. Draw two vertical lines with length 25.10mm and 7.37mm away from the edge of the circle. and cut extrude using "blind" and a depth of 30mm for both regions.
Next, viewing from the right plane, sketch a circle on the region we just cut. The diameter should be 8.38mm with a distance of 12.55mm from the upper edge and 14.95mm from the side edge. Make a blind cut that is 30mm.
On the right plane, make straight lines on both sides that are 15.05mm. Make a vertical line that is 28.74mm to connect the two lines. Draw a circle that has a 14.37mm radius and align it to the circle in the center already. Trim it to make a half circle. Cut extrude through all the ramp-shaped figure in the bottom of the part to leave a rounded edge.
After, viewing from the back plane, sketch two vertical lines with the length 25.10mm and 7mm from the center. Make a blind cut with depth of 35mm.
On the right plane, sketch a circle on the right part with the center 17.24mm away from the left edge of the part blind cut extrude through all to create a circle
On the right plane, repeat the ramp-shaped figure on the left side of the part.
Step 4: Create the Lever Arm/Handle on SolidWorks
On the front plane, sketch a circle with a diameter of 28.75mm at the origin. Boss extrude it 275mm.
Next, go to the back plane and sketch two vertical lines with the length of 25.10mm with a distance of 7mm away from the center. Extrude the two lines so that there is a gap in the middle with extrusion dimension of 35mm.
On the part we just extruded, sketch a circle with a diameter of 8.40mm with a distance of 17.76mm from the center of the circle to the edge and 12.56mm from the bottom of the part. Cut extrude through all to create a hole.
On the right plane create a short line with the length of 9.24mm that connects with the very left of the part. Draw an arc with a radius of 30mm. Then, draw a vertical line that connects the other end of the arc with the length of 76.39mm. After the sketch is complete, sweep the sketch.
After, fillet the top of the part we just swept 10mm.
Lastly, on the right plane, make straight horizontal lines on both sides of the part with the hole we created that are 17.78mm long. Make a vertical line that is 25.10mm to connect the two lines. Draw a circle that has a 12.56mm radius and align it to the circle in the center already. Trim it to make a half circle. Cut extrude through all the ramp-shaped figure in the bottom of the part to leave a rounded edge.
Step 5: Create the Arm Rest on SolidWorks
On the front plane, sketch a rectangle with a height of 170mm and length 195mm and make a blind extrusion 10mm.
*After Assembly, use the cavity feature to create the indents on the rectangular prism
Step 6: Create the Gear on SolidWorks
To begin the gear, create a new sketch on the front plane and draw two circles from the same point with the diameters of 25.40mm and 31.75mm. Then, boss extrude using a blind extrusion at 30mm.
Once the extrusion is done, create another sketch on the front plane and draw another circle with diameter 31.75mm and extrude 20mm.
Next, sketch on the front plane a circle with diameter 100mm and extrude it 12.70mm.
On the top of the part we just extruded, draw an equilateral triangle with sides 30mm. Extrude the triangle 12.70mm.
Once the extrusion is finished, use the circular pattern feature to have 20 uniform triangles all around the part. Then, fillet all the edges of the triangles.
On the front plane, sketch another circle with diameter 100mm and extrude it 13.97mm.
To create the hole in the middle of the gear, sketch a circle on the back plane with the diameter 27.94mm and cut extrude up to surface.
Step 7: Create Pawl on SolidWorks
On the front plane, draw a vertical line with length 2.07 inches. After, draw an arc with the radius of 0.40 inches connecting with the bottom of the vertical line. Also, draw a horizontal line connected with the top edge of the vertical line. Using smart dimensions, click the top edge and then vertical line and set the angle to be 78.00 degrees.
After the angle is set, draw another vertical line that connects with the slanted line with a length of 2.14 inches. Then fillet the edge of this line with the horizontal line with a radius of 0.28 inches.
Once the sketch is complete, boss extrude using a blind extrusion 0.5 inches. To create the hole in the middle, sketch a circle that has a radius of 0.12 inches at the center of the part and use cut extrude through all.
Step 8: Create Direction Knob on SolidWorks
On the front plane, sketch a vertical center line. Then, at the top of the center line, sketch an arc with a radius of 10mm. Then, on both sides draw slanted lines with the length of 18.26mm. Then, draw an arc on both sides with radius 5mm. To connect both sides, draw another arc with radius 18mm. Extrude the sketch using blind extrusion 12.70mm.
To create hole, sketch a circle with diameter 5.90mm that has the center 8mm away from the origin. Use cut extrude up to surface.
Scale the part about centroid with scale factor 0.8mm.
Step 9: Create the Pipe Mount
In order to create the pipe mount that will attach the lever arm to the body of the gear, begin with a sketch of two circles. The inner circle should have the diameter of the PVC pipe so that it may slide easily around it therefore, it should be 1.3125 inches. The outer circle should be about 1.5 inches. Make sure the two circles are concentric and extrude the portion between the two circles by 0.5 inches. Then, sketch a rectangle that matches the bottom face of the outer casing of the gear. This would be a rectangle of 3.5 inches by 1.25 inches. Center this rectangle around the circle by setting the long edge of the rectangle to be 1.75 inches away from the center of the circle and the short edge of the rectangle to be 0.63 inches away from the center of the circle. Extrude the rectangle by 0.5 inches. Because some parts of the rectangle lie within the inner circle, cut extrude the inner circle to clear it. Next, from the top plane of the part, sketch a center line from the circle to the outer part of the extruded edge. From this center point on the extruded edge, sketch a rectangle that goes 0.2 inches to both sides. Extrude this small rectangle by 0.5 inches. Create a front facing reference plane through the center of the part and use the mirror function to create an identical extruded rectangle on the other side of the circle.
When 3D printing parts, it is always a good idea to scale everything slightly up so as to avoid interference when placing the part on the assembly. In this case, the entire part was scaled up by 1.05. Finally sketch two circles of 1/4 inch diameter set to be on the front face of the center of the part with one on the small rectangle and one on the side of the circle. Making sure the two circles are vertically related, they can then be cut through the entire part, cutting out four circles in total. These would be holes for which the bolts can be placed to connect the PVC to the main body of the gear casing.
Step 10: Begin Assembly on SolidWorks
First, insert all the parts that were created in the previous steps along with the off-shelf outer knob, screws and nuts, making the wheelchair body the base component.
Begin by mating the body and the gear by clicking the edge of the gear and the edge of the body and use a concentric mate. Then, click the face of the gear and the body to create a coincident mate.
Then, mate the body and the direction knob by clicking the face of the direction knob and the body to make a coincident mate.
Now, mate the outer knob and the wheelchair body by clicking both the face of the outer knob and the body to create a coincident mate.
Create a concentric mate by clicking the face of the body and the face of the outer knob.
Then, make a concentric mate by clicking the face of the direction knob and the edge of the body.
Now click the faces of the body and the pawl to create a coincident mate and repeat for the other pawl.
Create tangent mate by clicking the face of the direction knob and the pawl and repeat for the other pawl.
Next, create a coincident mate by clicking the face of the body and the outer case and make a concentric mate by clicking the face of the body and the edge of the outer case. Then make the face of the body and the face of the outer case parallel.
Create a limit angle that has a maximum value of 78 degrees and a minimum value of 35 degrees for the face of the body and the face of the pawl and repeat for the other pawl
After, mate the joint and the body by clicking the face of both to create a concentric mate. Then create a centered width mate for both faces of the joint and the body.
Then, create a concentric mate for the edge of the lever arm and the edge of the joint. Create another centered width mate for both faces of the joint and the lever arm.
Make another concentric mate for the face of the joint and the screw. Then, create a tangent mate by clicking the face of the joint and the face of the screw.
On the right plane, sketch two axis lines for future mating reference with the first line being where the body meets the joint and the second one being where the joint meets the lever arm.
Next, create a concentric mate by clicking the face of the lever arm and the second screw. Once mated, create another tangent mate with both the face of both components.
With the first axis drawn previously, mate the edge of the first nut and the axis to create a concentric mate.
Use a coincident mate for the face of the first screw and the first nut and repeat for the second screw and nut.
Make a concentric mate with the edge of the second nut and the second axis.
Create another concentric mate with the face of the body and the external face of the first screw. In addition, make a coincident mate for these parts.
Make a concentric mate for the face of the pawl and the external face of the third screw.
Create coincident mate with the face of the body and external face of the third screw.
Next, create another concentric mate by clicking the face of the outer case and the external face of the third screw and make them coincident.
Make a concentric mate by clicking the face of the body and the face of the pawl and make them coincident. Repeat for the other pawl.
Make a concentric mate by clicking the face of the direction knob and the outer knob.
Lastly, mate the face of the body and the edge of the direction knob to create a concentric mate.
Step 11: Order Parts From McMaster-Carr
Order the plastic two arm knob (outside knob), alloy steel shoulder screw, steel hex nuts, and cable ties from McMaster-Carr. The item numbers are 65035K14, 92981A205, 90592A016, and 70215K61, respectively.
Step 12: Obtain Parts From Hardware Store
At a local hardware store, obtain the following:
- 18" x 24" x .220" acrylic sheet
- Clear adhesive (E6000 Adhesive)
- 1" PVC socket cap (2)
- 1" x 10' PVC plain-end pipe
- 1" PVC 90-degree elbow (2)
Step 13: Manufacturing the Parts
3D Printed Parts: Prepare the SolidWorks parts and converted them into STL files. From there, put the parts into the Makerware software and lay out of parts needed to be printed (shell of the body, gears, mounting piece, pawls, direction knob, arm rest indents*). If the parts do not fit onto the bed of the printer, wait to reprint again. When printing, be sure to add supports and rafts in order to prevent the prints from failing.
Laser Cut Parts: Using the 18" by 24" acrylic, the front and back plates of the outer casing of the body can be manufactured. This can be done by taking the front face of both plates on SolidWorks and saving them both as a DWG file. These can then be uploaded to the laser cutting software (in this case Epilog) in which their orientation can be set up as shown by the image. Two of each will be cut out of the acrylic, and from the remaining material, two rectangles will be cut. The rectangles will serve as the armrests.
Hand Cut Parts: Take the pipes and cut them into the different lengths (two of 4.5 inches for the handle, two of 4.5 inches for the joint, two of 6.5 inches for the lever, and two of 13.25 inches for the arm). From there, cut the 13.25 inch arm pieces on one end (30 or 35mm) down the middle of the other side of the pipe and drill a 1/4" hole 15 mm from the edges of the pipe. Cut and drill two of the 4.5 inch joint pieces in the same fashion but on both sides of the joint PVC pipe. Do the same (cut and drill) to the one side of the lever arm, 6.5 inch, pipe.
*Arm rest indents or the entire arm rest in the previous step may be used.
Step 14: Put Together All the Parts
Assembling the body:
Take the laser cut outside body pieces and the 3D printed shell pieces. Take one side of the outer casing and glue the shell pieces accordingly to the edges of the casing. Afterwards, take a rubber band and wrap it around the two pawls. Place the pawls in their respective locations and use the partially threaded bolt and place it through the hole of the body and the pawls. Afterwards, take the direction knob and the plastic knob. Place the plastic knob through the outer casing and twist the two together with the outer casing in between the two. Finally place the gear into its respective hole and place the top lid of the outer casing onto the gear and glue the shell to the top outer casing. Let it sit and dry. Remember to also secure the two partially threaded bolts with the hex nuts after placing and gluing the top lid to the shell.
Take the 6.5 inch lever PVC pipe and glue it to the bottom face of the body. From there, let it sit and dry. Take the mounted piece and slide it though the pipe until it is laying flat on the bottom face of the body. Take a 1/4 inch drill bit and drill the holes onto the pipe and through the body in its respective places. Secure the bolts with a hex nut.
Assembling the Arm Rest:
With the arm rest, simply place and glue the indents onto the 4 corners of the arm rest. Then drill two holes (5/32'' holes) on each side of the indents and place zip ties through them. The larger indents can then be aligned with and ziptied to the lever arm 13 inch PVC pipe. The smaller indent should align and later be attached to the arm of the wheelchair before use.
Assembling the Lever Arm:
Place the cap on the 4.5 inch handle pipe and place the elbow securely on the other side. With the other opening of the elbow, place the 13 inch arm pipe and connect it to one side of the joint (4.5 inch pipe) with a shoulder bolt. On the other side of the joint, take another shoulder bolt and join it with the (6.5 inch pipe) lever arm piece. Take a hex nut and secure the shoulder bolt. Because the shoulder bolts are partially threaded, the joints in which it is attached may be flimsy. In order to make the joints more tight and secure, place about five zipties around each shoulder bolt to tighten each joint.
Step 15: Iterative Testing
To test, make sure to get access to one of the wheelchairs.
Attach the lever arm to the wheel. Make sure parts fit where they're supposed to go, and make sure certain parts are parallel to respective parts of the wheelchair, like the arm rest. Make sure the holes drilled into the aluminum pipe and the body of the lever arm are aligned. If parts are disproportional, then go back and make some dimension changes.
Once the dimensions and relations are all correct, have a tester sit on the wheelchair and use the lever arm. As shown on the free body diagram, the tester will push forward horizontally to create a diagonal force which would be used to create a torque and propel the wheelchair forward. Analyze any problems: flimsiness of the joint, excess or lack of horizontal space, parts breaking etc.
Analyze problems and redesign again.
In our prototype, the wheelchair moved, but at a slow pace. The body part didn't finish gluing on time, so the lever arm broke during our test run. In addition, the joint may have been too big and loose, and there may not have been a sufficient amount of horizontal space and movement on the lever arm, both of these restricting the amount of force exerted per push.
Step 16: Contributions Page
Individual Contributions for Support System
Project Manager: Sophia Ynami 12732132
- The project manager, Sophia Ynami, was responsible for making sure every member of the group was held accountable for their respective duties and that all tasks were completed in a timely manner. I helped in the final assembly process as well as tested and made adjustments to the device before the final run.
Manufacturer: Yvonne Szeto 94326050
- The manufacturer, Yvonne Szeto, was responsible for getting the different components ready for assembly. I was responsible for getting the raw materials laser cut, drilled, and 3D printing different parts. I also assembled the different components together.
Materials Engineer: Willis Lao 15649487
- The materials engineer, Willis Lao, was responsible for deciding what materials to use for each component of the project and ordering/picking them from McMaster Carr/Home Depot. I also contributed to the Instructables by writing the introduction, cost analysis, the step by step process of creating parts, and the assembly.
Tester: Matthew Maravilla 25352925
- The tester, Matthew Maravilla, was responsible for overseeing and analyzing the iterative testing method, including testing the lever arm and reporting dimension or part changes to be adjusted. I also was responsible for the outline and the majority of the Instructables.
Lead Designer: Anthony Cheuk 30511803
- The lead designer, Anthony Cheuk, was responsible for coming up with a feasible design while taking into account the different materials that could be used and prepping the files and design ready for manufacturing (3D printing and laser cutting).