Introduction: Fulcrum Fabrication Lever Driven Wheelchair
This Instructables is the cumulative work of Fulcrum Fabrication during BME60C at UCI. Group members include Justin Perrizo, Meghan McDermott, Ehsan Alipourjeddi, Silin Cai, and Nasser Moreno. This project is in collaboration with the Free Wheelchair Mission and these designs may be utilized in the wheelchairs that Free Wheelchair Mission give away in developing nations.
Step 1: Research and Objective
Statement Market Proposition
At least 2% of developing country's population of over 6 billion people require wheelchairs though less than 10 % have access to them. Everyday 148 new people need a wheelchair and do not have access to one. The issue today is that very few people in 3rd world countries get access to wheelchairs and those that do have them, have difficulties riding over the rough terrain they live around. Our goal is to design a lever system to facilitate a person’s mobility through harsh terrain that is affordable and easy to use so that people from around the world acquire the help they need. (1)
Step 2: Base Plate
Simplicity was our goal when designing our parts. Therefore, all of our parts are simplistic, yet rigid and durable to ensure their dependability in developing nations. It is our goal to output a product that works well and is easily repairable, should repairs become necessary.
The base plate is the main fixture points for all other parts and secures the lever onto the frame of the wheelchair.
All dimensions are in mm.
Step 3: Base Plate Directions
1. In order to create the base plate, create a new part in millimeters. Then, from the origin, create the above left sketch. Extrude that piece 10 mm.
2. On the left most vertical line of the first sketch (the 25 mm line), create the above right sketch with the specified dimensions. Extrude that piece by 10 mm away from the extrusion from step 1. Merge the two parts during the extrusion.
3. The above part is now complete. However, a left side base plate is also needed. To convert to a left side base plate, just flip the orientation of the original part. The body of the base plate should now be on the right side of the part as shown above.
Step 4: Base Plate Drawing
Step 5: Hinge Bracket
The hinge bracket connects to the base bracket and holds both the lever and the gear cover.
Step 6: Hinge Bracket Directions
1. Open a new part. Create the following sketch, but separate the sketch into two parts, the rectangle and the bracket arm. Follow the dimensions provided in mm.
2. Extrude the bottom rectangle by 13.5 mm.
3. Extrude the rounded bracket arm by 3.5 mm in the same direction as the extrusion in part 2.
Continue to next step
Step 7: Hinge Bracket Directions Cont.
4. Create a plane at the end of the bottom rectangular extrusion and them mirror the entire part across this plane, as shown in the left image.
5. Create the following sketch on the top portion of the rectangular base (right image). Create two 5mm hole across the midline, 10 mm from the ends.
6. Convert those holes into M5 normal fit Counterbores for an ANSI B184.108.40.206M hex bolt using the Hole Wizard tool.
Step 8: Hinge Bracket Drawing
Step 9: Lever Arm
The lever arm propels the wheelchair forward and backward.
Step 10: Lever Arm Directions
1. To create the lever arm, first create a new part and set the units to MMGS. Then create the sketch below with the following dimensions. This will be a vertical piece of 145 mm in length, a horizontal piece of 200 mm in length, and a 300 mm vertical piece.
2. Exit that sketch and open a new sketch. Then, using either the bottom or top endpoint of the sketch drawn in the previous step, draw a circle with its center at the endpoint and perpendicular to the line. Also make sure that the circle is coincident to the endpoint. The diameter of this circle will be the thickness of the lever arm. Our lever arm outer diameter is 3/4 inch. (Note: this lever arm will be filled, while in practice, this part should be hollow.)
3. Use the swept boss/base feature and check sketch profile. Then, select the circle that you just drew as the sketch profile and the sketch drawn in step 1 as the sketch path. You will obtain the following part.
Continue to next step
Step 11: Lever Arm Directions Cont.
4. Finally, we need to make the holes at the bottom of the lever, where it will attach to the hinge bracket. To do this, first create a reference plane. Set the reference face to be the edge of the cylinder where you want to put the hole and set the relation to tangent. Then, set the secondary face to be either the front, side, or top plane. This depends on which axis you drew your initial sketch on. If you drew it on the x-y plane like I did, you will use the right plane as the secondary reference. If you did not draw it on the x-y plane, select the plane that will be parallel with the reference plane you are trying to insert so that it looks like the image below.
5. Click the green check mark and you should then obtain a plane that is tangent to the edge of lever cylinder and parallel to the front plane. (Or the side/top plane depending on where your sketch was drawn). The image below has this new plane highlighted and shows the front plane going through the middle of the part.
6. Now we can create the holes onto the lever arm. Create a sketch on the reference plane and draw a circle and dimension it appropriately. Our purposes will require a hole at 10 mm from the bottom of the 145 mm piece and another hole at 20 mm from the bottom of that same piece. These holes are 5 mm in diameter, plus a clearance of .1 mm.
Step 12: Lever Arm Drawing
Step 13: Gear
The gear moves the wheels of the wheelchair by being driven by the pawls and the lever.
Step 14: Gear Directions
1. Make a new part. Create a new sketch of two concentric circles of differing diameter. The inner circle is 28 mm and the outer circle has a diameter of 150 mm.
2. Create a third circle that is vertical to the inner circle and 40 mm above the center of the inner circle. Give this third circle a diameter of 10 mm. After, using the circular sketch pattern located under the linear sketch pattern button, create a pattern with 12 instances. . The first circle should be the only one fully constrained, so add a angular constraint by using the fully dimension button located under the display/delete relations tab. This is what your part should look like until now.
Continue to next step
Step 15: Gear Directions Cont.
3. Go to the edge of the larger circle and drag a line down towards the center and create a length of 10mm for the line.
4. Draw another line 20 mm away from the previous line. Draw out a curve that then connects to another straight line like the one you just made.
5. Using the circular sketch pattern tool, click on the three lines that compose the cut you want to make and create ten of the pattern. Next, using trim entities, trim the sides of the circle that cover the cuts you want to make, and the program should automatically create the pattern seen above.
Step 16: Gear Drawing
Step 17: Pawl
The pawl fits into the teeth of the gear to push the gear forward and backward.
Step 18: Pawl Directions
1. First, create two center lines that make an axis through the origin. Draw a circle above it with a 20 mm diameter and make it coincident with the bottom center line. The origin of that circle should be on the vertical centerline. Next, draw a circle within the first circle you drew with the dimensions 6.35mm and make it concentric to the larger circle.
2. Sketch a line going roughly from the bottom of the larger circle to an arbitrary space to the left. With a tangent mate, mate the line and the outer edge of the larger circle. Using your smart dimension tool create a 16 degree incline from the line you drew to the bottom horizontal centerline. Then insert another line, tangent from the top of the larger circle, and horizontal leftward. Dimension this to be 54mm. Now, to create the front bit, from the angled line draw a curve with a radius of 30 that ends right below the length of the 54 mm line. Connect the two edge points with a vertical line. To constrain the curve, use the tangent mate between the curve and the angled line. To constrain this part, define a length of 40 mm from the intersecting point between the curve and angled line and the center of the circles.
3. Extrude the entire sketch 10 mm.
Step 19: Pawl Drawing
Step 20: Gear Cover
The gear cover allows the wheelchair to go forward and backward by blocking the pawl from touching the teeth of the not desired direction.
Step 21: Gear Cover Instructions
1. This is the first step to creating the gear cover. A rectangle is created on the top plane, using the rectangle sketch tool, and dimensioned in accordance with the dimensions desired for the main surface of the cover. This particular rectangle will be the first back section of the cover.
2. Create a new sketch on the right plane. To create the gear cover I created a pathway for the initial shape to follow by using the arc tool, in order to later use the sweep function. The length and curvature were determined based on the radius of the gear and to the extent we wished to cover the sections of the gear. In total the cover will be roughly covering 144 degrees of the gear.
3. Then using the base sketch and the pathway a sweep is created. Using sweep allows for the curvature to be followed in a more accurate pattern. As this is only the back section of the cover it only extends to about 50 degrees in length in accordance with the overall gear.
Step 22: Gear Cover Directions Cont.
4. Then in order to move forward with the next middle section a new plane is created off of the end of the first sweep by clicking reference geometry and clicking on the edges of the base sketch to create a new plane. On this newly created plane a section double the width of the base sketch is created using the rectangle tool again in order to create the middle section which the pawls will cross over in order to enable the switching of directions.
5. The pathway for the next sweep is then created, again on the right plane using the arc tool. The middle section is slightly smaller than the back and front extension to allow the pawls to be in action for the particular direction longer.
6. Utilizing the sweep function the middle crossover section is created by selecting the new sketch and pathway for it to follow. It cover 44 degrees of the main gear circumference.
Step 23: Gear Cover Directions Cont.
7.Then another plane is created to build the last section off of the end of the second sweep, once again by clicking reference geometry selecting plane and then selecting the edges of the end sketch to create the new plane. The last section of the gear cover is the front extension, which is the mirror image of the base sketch flipped across the center of the crossover section. Or you can just create another rectangle with the same dimensions as the base sketch but placed on the other end.
8. This is the pathway for the last final sweep created on the right plane using the arc tool, the front extension of the cover. The pathway also covers like the back pathway 50 degrees of the gear circumference.
9. Using the sweep feature extend the last section of the cover.
Step 24: Gear Cover Directions Cont.
10. Sketch off the back of the gear cover a small lip to later be extruded in order to attach onto the rest of the assembly. Use the arc tool and line sketch tool to create this lip sketch.
11. Use the extrude feature by selecting the sketch to extend the sketch outward to satisfy a lip to reach out past the gear and be attached to the rest of the assembly.
12. On the front plane sketch a rectangle to match the main feature of the lip you just previously created. By clicking on the edges of each sketch using the shift button you can create relations in order to constrain the sketch without using scalar dimensions.
Step 25: Gear Cover Directions Cont.
13. Using the extrude function and selecting the to surface feature connect your last rectangular sketch to the lip previously created. This creates a block feature that can be attached back to the full assembly.
14. On the top plane sketch an L configuration using the line tool to later be cut out of the the previously created block. This L configuration will create room for the gear cover to be attached and not create unnecessary friction with the gear.
15. Utilizing the cut extrude feature select the sketch and remove the L configuration from the block.
Step 26: Gear Cover Directions End
16. Using the fillet feature select the inner edge of the gear cover to remove rough edging and create a rounded edge.
17. Create a circle using the circle sketch tool and dimension it. This circle will later be used to slide a bolt through.
18. Using cut extrude tool cut out the circle by selecting the sketch using the blind setting to pass it all the way through the feature.
Step 27: Gear Cover Drawing
Step 28: Gear Attachment Piece
The Gear Attachment Piece slides into the hub of the wheel and fixes the gear to the wheelchair. This allows the wheels to spin when the gear is propelled forward.
Step 29: Gear Attachment Directions
1. Make a new part. At the origin, sketch two circles of 12 mm and 20 mm that are concentric. Extrude these pieces 2 mm. This should give a hole through the center.
2. On the top face of that extrusion, sketch two more circles from the origin of 19 mm and 25 mm. Extrude this sketch 13 mm in the same direction as the extrusion of step 1.
3. On top of the face of the step 2 extrusion, sketch two circles of 25 mm and 120 mm. Extrude this sketch 10 mm.
Step 30: Gear Attachment Directions Cont.
4. On the face of the step 3 extrusion, sketch a 10 mm diameter circle with vertical relation to the origin and 40 mm above the origin.
5. Using the circular pattern tool, make a circular pattern of these holes with 12 instances.
6. Using the extruded cut tool, cut the circular pattern sketch through all.
Step 31: Gear Attachment Drawing
Step 32: Step by Step Assembly of Whole Model
Step 33: Final Assembly
This is what the final assembly should look like. The gear attachment can be tied to the gear with nuts and bolts or with high tensile strength rope.
Parts used for this assembly include:
* Off the Shelf Part
Base Plate Bracket (Right and Left)
Hinge Bracket (2)
Gear Cover (2)
Gear Attachment (2)
*M12 x 1.75mm Thread, 160 mm Long, Zinc-Plated (2)
*M5 x .8mm Thread, 35 mm Long, Alloy-Steel Socket Head Screw (4)
*M5 x .8mm Thread, Class 10, Steel Nut (4)
*12 mm Shaft Diameter Permanently Sealed Ball Bearing (2)
*19 mm OD for M12 Bolt, 10 mm Long, Unthreaded Aluminium Spacer (2)
*10-32 Thread, 2-1/4'' Long 18-8 Steel Screw (4)
*10-32 Thread, Steel Nylon-Insert Locknut (4)
*8 mm OD for M5 Bolt, 14 mm Long, Unthreaded Aluminium Spacer (2)
*3/4" OD, 1/8" Wall Thickness, 6061 Aluminium Round Tube (6 feet)
*10mm Width Plywood (2.5 ft x 2 ft)
*Dry-Environment Polypropylene, 6" Long Cable Ties (20)
Step 34: Final Assembly Drawing
Step 35: Final Assembly Drawing Part II
Step 36: Prototype Material Choice
Our lever arm design is an original design. Therefore, to allow for a quick and accurate building of our part within in the time frame required, coupled with our groups limited expertise in manufacturing, we decided to 3D print all our self-created parts except the lever materials using ABS plastic.
As for the tubing, we wanted to be able to use a material that was very strong and durable, yet cheap and easy to cut. Therefore, we chose 6061 standard grade aluminium. For our off the counter parts we wanted to use steel because for the nuts, spacers and screws we needed very durable material to not break under heavy loads. The cable ties would be a cheap and easy way to mount the prototype gear to the base part. We just used the standard harsh environment so that it doesn’t easily snap.
Revisions to prototype for materials:
When we went to 3D print the gears, Fabworks would not print the gears, so we had to transition using high strength plywood so that we could keep rigidity but also efficient for the gear motion. Our original plan of welding the aluminum lever was out of our scope of expertise, so we decided for the prototype to by regular PVC joints to attach the cut levers together, which also gave it some additional strength.
To help account for these new material choices, putty was used to its form and malleability for the elbow joints, and epoxy was very efficient due to its high strength and fast cure times.
Step 37: Final Product Material Choice
The final material choice was dictated by using the CES software. Because the strength of the material is the most important factor in the intrinsic material itself, and with the fact that there is cost limit, this analysis was done. The material also needs to be rust resistant, so aluminum was the best material. In particular was Aluminum 1050A, H19. All of the custom designed parts will be this material, which minimizes the need for additional material to be purchased.
Step 38: Building the Prototype
Step 39: Building the Prototype Directions
1. First we 3D printed all of our Solidworks parts and sent in the order form for all the piping, screws, bolts, and nuts we need to complete the prototype.
2. The gear that was designed for this particular set up is too large to be 3D printed and therefore we selected to cut it out of wood. Therefore the gears were made later by first cutting the wood and processing it more to achieve our desired design.
Step 40: Building the Prototype Directions Cont.
3. The wood was then later then measured and marked for the cuts necessary to create the full gear. It was then cut with a coping saw in order to create the notches that are needed in order for the pawls to work correctly.
4. The edges of the wood were then sanded in order to remove any rough edges and make the gear more uniform if any imperfections created a possible obstructions to the vital function of the pawls in the gear.
Step 41: Building the Prototype Directions Cont.
5. Moving forward the gear need to be drilled. Therefore a center axis hole was drilled and using a tap the quarter inch holes vital to the design of our gear were also tapped. The quarter inch holes were used to stabilize the gear onto the wheel chair itself.
6. Then the large center axis hole itself needed to be sanded in order for a smooth fit of the bearing into the wooden gear.
7. After sanding the center axis hole the bearing was tapped into place.
Step 42: Building the Prototype Directions Cont.
8. Then we began the basic assembly of the 3D printed base plate and hinge bracket. They were assembled using two M5 screws and nuts in order to secure the pieces together.
9. Attach the hinge bracket and base plate configuration to the gear cover and then fit the overall configuration to the small 5.5" pipe on the bottom drilled hole.
10. Using JB weld putty put together the two larger pipes in descending order in an L configuration and leave to dry. After dry attach the small pipe with the base configuration to the second largest pipe using the JB weld putty parallel to the largest pipe.
Step 43: Building the Prototype Directions Cont.
11. Attach the pawls together using an M5 screw and then screw through onto the small pipe in the hole directly above the gear cover.
12. Gather gears to be attached using the large bolt as an axis through the bearing in the center of the gear.
* Don't cut yourself. (If you do, try not to bleed over the assembly).
13. Complete assembly by attaching to the wheelchair, currently using cable ties due to this still being a basic prototype phase.
Step 44: Cost Analysis
Total Tax was $9.71.
In addition to the 52 dollar cost for 3D printing (and reprinting of the gear cover and washers) , our total was $187.12, which was under the 225 prototyping budget.
Final Product Cost:
To account for our final cost of our aluminum Solidworks products, the the amount used was calculated using Solidworks (37.38 cubic inches for one side) , and from the price on material description the EDUpack software ($4560 per cubic meter), the total price for our self designed parts are $5.59.
For our off the shelf parts, we used
2 of the M12 x 1.75mm Thread, 160 mm Long, Zinc-Plated ($4.38),
4 of the M5 x .8mm Thread, 35 mm Long, Alloy-Steel Socket Head Screw ($0.67),
4 of the M5 x .8mm Thread, Class 10, Steel Nut ($0.29),
2 of the 12 mm Shaft Diameter Permanently Sealed Ball Bearing ($35.90),
2 of the 19 mm OD for M12 Bolt, 10 mm Long, 2 Unthreaded Aluminium Spacer ($8.18)),
4 of the 10-32 Thread, 2-1/4'' Long 18-8 Steel Screw ($1.29) ,
4 of the 10-32 Thread, Steel Nylon-Insert Locknut ($5.95),
2 of 8 mm OD for M5 Bolt, 14 mm Long, Unthreaded Aluminium Spacer ($3.34).
With a tax of $4.65 it becomes $64.65 for our off the shelf parts.The $64.65 plus $5.59 equals a total cost of $70.24 for a single non-mass produced set of wheelchair levers. This is 76 cents under the total allowable budget.
Step 45: Iterative Testing Method & Free Body Diagram
Free Body Diagram(Above Image)
Iterative Testing Method
(This Project ended in the prototype phase so further iterations of improvement were not processed through multiple prototypes.)
In terms of testing our individual parts, we subjected each part to a light stress testing consisting of bending and flexing each part accordingly. Upon first iteration, the gear cover proved to be too small and thus we tripled the size of the sweeps. Accordingly, due to the new size of the gear cover sweeps, the pawls were too short, but this was overlooked until race day. Thus, the gear covers were removed in an attempt to force the assembly to function. When assembled together, the 3-D printed base bracket proved to be too weak and snapped around the main loop hole. This resulted in assembly failure, resulting in inability to race. If the base bracket was made of a stronger material and the pawls were longer, then this assembly should have worked.