As Biomedical Engineers at Wheelchair Modders, we strive to “simply” improve lives. “Providing wheelchairs that are appropriate, well-designed and fitted not only enhances mobility, but also opens up a world of education, work and social life for those in need of such support” explains the World Health Organization on their website. In regions with gross national incomes per capita up to twelve thousand dollars, from a statistic by the World Bank website, the challenges of accessibility due to disability encumber a multitude of people. Susan Shore and Stephanie Juillerat note in “The impact of a low cost wheelchair on the quality of life of the disabled in the developing world,” how patients in the developing world experienced an increase in health and mood by 20% and increased independence by 11% after a year of using a gifted wheelchair. Our innovation? To “simply” improve the Free Wheelchair Mission’s Gen_2 wheelchair’s efficacy in providing freedom to patients in the developing world with lever arms.
Our method is driven by the parameters of the given environment. With socioeconomic disparities, the solution must be of low cost and high lifetime. With infrastructural disparities, the design must be robust and easy to repair in failure. With concern for patient livelihood, the design must exhibit a degree of additional efficiency in function of the wheelchair and concern for ergonomics. Other wheelchairs to facilitate freedom exist, but not under the same constraints. The Bounder is robust, but costs $14,000. The Freedom Chair is mobile, but too hefty for the inconsistently tight “urban” areas with cramped, sprawling buildings in the developing world. The NuDrive is another solution, but consists of a lot of custom, high quality material parts requiring high precision. So we “simply” designed for the developing world. Inspired by the ratchet we used to assemble the Gen_2 wheelchair, we devised a ratcheting mechanism of two ratcheting gears in opposing direction, allowing propulsion in both directions with parts that can be made in a simple workshop. Additionally, this allows the wheelchair to spin in place. Endowed with physiological knowledge, we “simply” decided on horizontal grip to direct strain on the pectoral and dorsal muscles, which are much stronger than the rotator cuff and other smaller shoulder muscles that are required to operate a vertical lever arm. The horizontal grip will be able to move up and down the lever arm to adjust for different torques, as well as be able to free-float if selected for a more natural motion when pushing the levers forward. Caliper brakes attached near the bottom of the lever arm will be used to stop the tires when needed and will be controlled via the horizontal grip for easy access to safety. Our market needs a minimalistic mechanism, which we deliver. Our market wants the comfort of easy repair on top of the comfort of our ergonomic, efficient approach. Our market on top of those chief concerns, gains an ability to easy modification and adaptation to environment with our solution. Our market needs the Simplever.
Step 1: Basic SolidWorks Functions to Know
In order to design the lever arm in SolidWorks, there are a few features you, the user, should know. The most common of which you will see in this instructable are: sketching, boss extrusion, hole wizard, and patterning. We have provided you with tutorial videos on how to do these basic functions using our first part (the snapping mechanism) as an example.
Step 2: Designing the Snapping Mechanism
To make the snapping mechanism for our lever, a base sketch of a circle is needed on the front plane and smart dimensioned to be 100 mm in diameter.
Then, an extrusion of that circle is made to give it a depth of 5 mm.
Make 12 holes, six outside and six inner holes, with the hole wizard.
Within the hole wizard, the ISO grade standard for a counter-bore head, as well as a standard Hex bolt grade C ISO 4016 is implemented. An M5 size head diameter fits perfectly with the plates, with a close fit for accuracy, and an end condition of through-all since the bolts should go through the width of the plate. There is one hole on the top of the plate, which is smart dimension'ed from the center of the hole to be 37.50 mm from the center of the plate. From there, the circular pattern option creates five more of same holes made via hole wizard, perfectly aligned along the sides of the plate. Within circular pattern, the face of the plate is the front plane with equal spacing as well as six instances (holes) that are 360 degrees apart and aligned on the plate.
The inner holes are made using the same method:
The hole wizard to create the same holes with the same conditions, but since this is an inner hole, the distance from the center of that hole to the center of the plate will be shorter (18.00 mm). The plates have a set tolerance of 0.05 mm by clicking custom size, adding diameter tolerance. Circular pattern option creates the other five inner holes of same dimensions and features with the same settings of choosing the face as the front plane with equal spacing for the holes, and six instances (holes) that are 360 degrees apart and aligned on the plate. Cut extrude adds the essential size extension of the inner, top hole so the hole is 10 mm in the shape of an oval for the plate to be exactly constrained. Lastly, one of the snapping mechanism's must fit through the axle of the wheel, so cut extrude helps with making a hole that is 15 mm diameter to encompass the axle.
Step 3: Snapping Mechanism (E-Drawing)
The e-drawing's of the snapping mechanisms consist of the standard A3 ISO sheet format. The standard views within the e-drawings are the top, front, right and isometric view. Dimensions are shown within each view to properly display relevant information, such as the diameter and width of the disk, the diameter and sizing of the holes, and the specifics about the ovals made (for exact constraint). The drawings are 26-point font for each text annotation, smart dimension, and the bill of materials. There are two snapping mechanism engineering drawings because one of them accounts for the wheel axle.
Step 4: Designing the Gears
Use the circle sketch tool to make a circle on the front plane, with the origin as the initial point. Be sure to select for construction before completing the sketch.
Now under the same tab, select the tool “smart dimension”. Specify the edge of the circle and dimension it to have a diameter of 90 mm.
Now select the line sketch tool and select the origin. From there, select the option “for construction” once again. Connect the origin and edge of the circle via line, and back in the opposite direction, so to have overlaid vertical lines, to allow proper extrusion to occur. For a new line entity, select the origin and connect with edge via arbitrary line.
Use smart dimension to set the vertical and arbitrary lines fifteen degrees apart, to correspond with the total twenty-four teeth of the gear to be made.
Create an L-shaped entity from the vertices created by the coincident points on the edge of the circle, then set the angle of the portions of the entity to be eighty degrees apart.
Now using the button “linear sketch pattern”, open the drop down menu to select the option “circular pattern”. Be sure spacing is set to “equal spacing”, instances are set to twenty-four, and degrees for spacing are set for the full three hundred-sixty.
Now that the sketch for the base feature is complete, extrude the gear’s main body by using “extrude boss”. Set thickness to 10 millimeters. Also, ensure that the proper inner contour is selected for extruding the gear.
With the base feature made, select the sketch tab again and select the front face of the gear body, using a point coincident with the origin to create a sketch of a circle. Now use smart dimension and set the setting under “Tolerance and Precision” to “Bilateral”. Enter the proper tolerances for the given hole size made. Now extrude the cut “through all” for the central hole.
Select the hole wizard tool from the features tab and select the counterbored m5 hole (find m5 by changing to ISO metric standards). From here, select the tab “positions” displayed in the same spot as the feature tree, then use smart dimension to position the hole eighteen millimeters away from the origin. From here, use the circular pattern tool to copy the hole a total of six times around the central hole.
Step 5: Gears (E-drawing)
Select button to make a part into an e-drawing in Solidworks. From there, select the A3 ISO format, upon which the three standard views in the format's default scaling (1:2) are input, along with an isometric view of the part. Select all the centermarks to be on, and mark the holes with bilateral tolerances, done to each type of hole, as there are different sizes present in the part. List the material in the title block (AISI 304), as well as the fasteners required for the part (Hexbolts M5x1.8x80, M5 nuts, M5 washers)
Step 6: Designing the Directional Lever
First, sketch the bottom portion of the lever to have three sketch entities:
two symmetric circles of radius 3.5 mm on top and bottom
lines to connect the circles' horizontal radii, that are 30 mm tall
Now extrude outwards 9 mm. Sketch circles on top of the circles of the last sketch and extrude outwards a further 10 mm.
Now select the plane where the circular features now lie, and continue the lines from the initial sketch a further 100 mm upwards, and end the top with a straight, horizontal edge. Extrude this sketch inwards (opposite of prior extrusions' direction) 19 mm
Select one of the narrow faces of the last feature. Atop the straight top edge, sketch a 30 mm by 30 mm square. Extrude to match the depth of the last feature made.
Step 7: Directional Lever (E- Drawing)
Select button to make a part into an e-drawing in Solidworks. From there, select the A3 ISO format, upon which the three standard views in the scale of 1:2 are input, along with an isometric view of the part. Select all the centermarks to be on for circular components of the part, and mark the circular protrusions with bilateral tolerances. Take note of all present and necessary dimensions of the part. List the material in the title block (Aluminum 3003 H14)
Step 8: Designing the Pawls
We begin creating the part by generating a base sketch. We do this by creating a circle and attach two tangent lines that we looped together into a trapezoidal shape. We added a circle concentric to the first one and another circle not to far off that will act as holes we will need for our assembly. Then we dimension the sketch appropriately to match the dimensions of the ratchet that goes along with this pawl.
Then we create a three dimensional version of the sketch by using “extrude boss” and selecting the thickness we want the pawl to have. We also used the extrusion from midplane in case we wanted to use the natural coordinate planes as reference planes in the future.
Now we draw a circle on the top plane, at the center of the trapezoidal portion of the pawl. This will serve as the base sketch for the spring holder needed for the pawl. We dimension it appropriately.
Finally we use “extrude boss” to create a 3D feature and apply the height we want for the spring holder and then the part is finished. We used extrude “from face” so Solidworks knew to extrude from the pawl and not the top plane.
Step 9: Pawls (E-drawing)
Select button to make a part into an e-drawing in Solidworks. From there, select the A3 ISO format, upon which the three standard views in the scale of 2:1 are input, along with an isometric view of the part. Select all the centermarks to be on, and mark the holes with bilateral tolerances, done to each type of hole, as there are different sizes present in the part. Take note of all present and necessary dimensions of the part. List the material in the title block (AISI 304)
Step 10: Designing the Housing Part I
Proceed to selecting the sketch tab, the tool “sketch”, and selecting the front face once prompted. Use the center rectangle tool to make an arbitrary rectangle. Select the smart dimensioning tool, and dimension the rectangle as displayed above, with a height of 150 mm and a width of 180 mm. Select the tool for sketching lines, select the option from the dropdown menu of centerlines, and proceed to construct center lines with the relations portrayed below. Though the centerlines are not necessary for this stage of the part’s design, it aids in gauging the design of the part, considering how it is designed around the other components of the gears, pawls, and levers.
With the fully defined sketch of the rectangle, one can now extrude the base feature of the box. Select the tool “extrude boss” and set the depth of extrusion from the sketch plane to be 60 mm.
Now with the box made, the shell feature tool can now be used to hollow out a large portion of the box to accommodate the gears and pawls. Set the thickness to 10 mm, and select “show preview” to again gauge the design’s relative proportions.
With a completed, fully defined circle, extrude to form a cylindrical protrusion. Set the depth to be 50 mm, reaching in the direction of the gap in the main box feature.
On the same plane referenced just prior (the interior front plane), create a sketch now using two centerlines, from which one can dimension the location of the protrusions for the pawls to lie on. Dimension for one protrusion, then use mirror entities to copy it about the vertical centerline.The radius of the circle is 7.5 mm, laterally 52.6 mm away from the vertical centerline and with a vertically 29.5 mm away from the horizontal centerline. Extrude the entity just sketched “through all”. Since the entity is mirrored, changing one will change the other, and this also carries into the properties of features as well
Step 11: Designing the Housing Part II
Using the axis directory on the bottom left corner of the Solidworks workspace, select the green y-arrow to change to a top view of the housing unit. Once there, mark the horizontal centerline, create two rectangles on either side of the centerline. Give them a horizontal dimension of 35 mm and a vertical dimension of 12 mm. Place both horizontally 25 mm away from the center line. The one to the right of the centerline is placed 20 mm away vertically from the top edge, and the top edge of the other rectangle lines up to the bottom edge of the rectangle on the right.
From here, extrude cut, selecting both of the contours independently and selecting “up to next” to ensure that the hole only goes through the shell, not the entire box.
Now return to viewing the box from the top. At the corresponding edges to each of the rectangular holes in the depiction below, sketch squares with a side length of 10 mm. Ensure the presence of one coincident relation for each of the squares to fully define them.
Extrude the sketches with 10 mm of depth upwards, yielding cubic protrusions atop the housing unit at this stage.
Use the “fillet” tool under the features tab to round the inner aspects of the cubes, allowing easier movement for the directional levels or any of its possible substitutes.
Step 12: Designing the Housing Part III
Having found dimensions from the bottom portion of the lever arm itself, this sketch is supposed to have these dimensions plotted to aid in placing holes for bolts to traverse and unite the separate components.
Now dimension for equidistance relative to the housing unit’s centerline and the bottom portion of the lever arm as follows, to ensure proper alignment of holes and thus nuts and bolts to hold the parts together. Place points at each location to later accommodate the hole wizard features.
Step 13: Housing (E-drawing)
Select button to make a part into an e-drawing in Solidworks. From there, select the A3 ISO format, upon which the three standard views in the scale of 1:2 are input, along with an isometric view of the part. Select all the centermarks to be on, and mark the shafts with bilateral tolerances, done to each size of shaft, as different configurations are present in the part. Take note of all present and necessary dimensions of the part. List the material in the title block (Aluminum 3003 H14)
Step 14: Designing the Lever Arm
A rectangle was sketched as the base; the base was extruded to create a long rectangular prism.
On the top of the small face of the prism, a rectangle with a small extension to one side was sketched; the sketch was then cut-extruded to make the prism hollow.
A small circle for a hole was sketched and a cut was extruded. A linear pattern was used to repeat the holes from along the length of the lever.
A small circle was sketched and cut-extruded near the top of the lever for the eyebolt.
Another circle was sketched and cut-extruded midway towards the bottom of the lever for the other eyebolt.
A rectangle was sketched on the face of the lever and extruded to hang over the tire.
Linear pattern was used to copy the extension to the other side of the lever.
A circle was sketched and cut-extruded through all for a threaded rod.
A rectangle was sketched and extruded on the bottom of the lever to provide a solid bottom.
Four M5 tapped holes were added with the hole wizard.
Step 15: Lever Arm (E-drawing)
Select button to make a part into an e-drawing in Solidworks. From there, select the A3 ISO format. Select all the centermarks to be on, and mark the shafts with bilateral tolerances, done to each size of shaft, as different configurations are present in the part. Take note of all present and necessary dimensions of the part. List the material in the title block.
Step 16: Designing the Handle - Main Body
Sketch circle and extrude base. Create parallel reference plane. Sketch rectangle on plane and extruded loft. Sketch identical rectangle and extrude boss. Sketch two circles and extrude boss. Thread bottom cylinder. Fillet top cylinders and rectangle edges. (first 3 pictures)
Create three reference planes. Sketch circle on plane 1 and extrude base. Sketch a circle on planes 2 and 3, each, and extrude loft. Sketch hook profile then extrude sweep. At bottom of cylinder, sketched larger circle and extruded boss. Sketch circle and extrude base. Sketch smaller circle on face of base and extrude boss. Add 0.25 in diameter hole with hole wizard, thread the hole. Fillet edge of the base cylinder. (fourth picture)
Sketch circle with smaller concentric circle and extrude base. Sketch smaller concentric circle on face of base and extrude boss. Sketch rectangle on face and extrude boss. Sketch circle of same size as concentric circle in (1) and extrude boss. (last picture)
Step 17: Designing the Handle - Rotating Grip
Sketch two concentric circles and extrude base
Sketch small rectangle on face of base and extrude cut
Step 18: Designing the Handle - Spring
Sketch circle and create helix
Sketch small circle on reference plane and extrude sweep along the helix
Sketch two rectangles and extrude cut to shorten spring
Step 19: Designing the Handle - Sub Assembly
Added all parts to the assembly
Concentric mated the spring, adjustment fork, grip casing, rotating grip, and button end
Parallel mated spring, adjustment fork, and button end
Parallel mated button end to the adjustment fork
Tangent mated button end to adjustment fork
Coincident mated button end to spring
Coincident mated button end to adjustment fork
Coincident mated the grip casing to the spring, then to the rotating grip
Concentric mated the brake hook to the small hole on the grip casing
Coincident mated the brake hook to the small hole on the grip casing on the far side from the button end
Step 20: Handle (E-Drawing)
Create an exploded view of the assembly beforehand, then click the button to turn it into an e-drawing. Select the A4 ISO format and show all present and relevant dimensions. Add a bill of materials in the upper righthand corner, delete the description column and add a new column to the right. Specify the property of the newly added column as the "Material" of each component in the assembly. Use the balloons to number off the parts in the exploded view. Specify tolerances needed for the holes/shafts in the title block below.
Step 21: Designing the Caliper Brakes - Side 1
The first step is to create the base sketch on the front plane. (The base sketch is modelled after the general appearance of most side pull caliper brake systems.) When creating the base sketch, start by drafting the general shape of the caliper. This entails utilizing the line sketch tool as well as the arc sketch tool. Then, incorporate your geometric relations. Prominent relations in this sketch are concentricity between the arcs. Lastly, incorporate approximate dimensions (which can always be scaled up or down, as we will see later).
Next, transform the base sketch into a 3 dimensional feature. This can be done by clicking “extrude boss” and then clicking the face of the base sketch. You will be prompted to enter the thickness of the extrusion. We chose 8.7 mm, based on the dimensions of our lever arm.
Now, create the holes in the caliper. We’ll start by making the hole for the brake pad. Here, we utilized the hole wizard and set a counterbore M5 hex head bolt hole. (We positioned the hole 8.8 mm above the bottom curvature and 4.4 mm from the vertical edges.) Most importantly, don’t forget to tolerance your hole. This comes in handy when bringing your CAD into the the physical world. For this case, as the brakes are a reference part in this model, we recommend a 0.001 mm tolerance for all the holes.
Utilizing similar techniques as step 3, create the holes for the mount and the hole for the side pull mechanism . In this case, we utilized a M10 tapped hole for the mount because we assume a simple rod to protrude through. Then, we utilized an M6 tapped hole for the side pull hole because we want to allow for flexibility in this reference design. (Different caliper systems use different rods or bolts in this mechanism.) Again, remember to tolerance your holes, 0.001 mm is still an acceptable tolerance.
Step 22: Designing the Caliper Brakes - Side 2
Similar to the Caliper 1, we begin by creating a base sketch on the front plane. The sketch is similar to Caliper 1, with the exception that there is an extrusion on the upper left and that the extended part of the arcs are omitted from the right. Again, start by creating the general sketch, extrude the sketch, and create your holes.
Step 23: Designing the Caliper Brakes - Brake Pads
Start with a simple base sketch on the front plane. Here, all you need to do is create a rectangle with the line sketch tool. Ensure that you have two vertically constrained relations and two horizontal relations.
We extrude boss the sketch to a thickness of 4 mm.
Next, go to the “Insert” tab and roll over to “Reference Geometry” in order to create a reference plane. Then, select one of the larger faces of your box and a reference plane will be created. Place a 4 mm distance between your box and the reference plane. This plane will allow us to create a sketch of a larger rectangle on your reference plane.
Then, utilize the boundary boss feature in order to fill in the space in between the reference plane and the box. This feature will expand the brake pad so that it begins at the smaller box and slopes out to account for the size of the larger rectangle sketched on the reference plane.
Lastly, create an M6 tapped hole in the center of the brake pads. You will want to do this on the side opposite of the reference plane. Remember to tolerance your hole.
Step 24: Designing the Caliper Brakes - String
First, create a a 2mm circle and extrude boss it to the length of the lever arm.
Then, create a loop from one end of the extruded cylinder. This loop is then utilized as a reference for the sweep function that will allow the string to curve in on itself.
Create a similar loop on the other end by also using the sweep function.
Note: This string will not be shown in the subassembly of the caliper brakes because it is to be incorporated into the main assembly.
This string is a prominent feature of our design because as it remains vertical in a fixed distance, the user can adjust the horizontal handle to any position she or he pleases. At any of those positions, pushing the handle's button will cause tension on this string, activating the caliper brakes.
Step 25: Caliper Brakes - Sub-assembly
The first step in assembling the caliper brake system is to make the mounting hole on Caliper 1 and Caliper 2 concentric and coincident. In this way, it’ll allow for the two parts to rotate about one another while ensuring that the calipers do not separate.
The next step is to insert the bolts into the side pull mechanism. This part of our model is what deviated the most from an actual caliper brake system. In most cases, there are parts in this section that are most likely not just a bolt, but for our purposes, this shall suffice.
In order to assemble this section on CAD, simply create the (M3) bolts concentric with the holes, then make the inner face of the bolts coincident with the caliper faces.
The last step is to attach the brake pads to the calipers. Make the holes on the calipers concentric with the holes on the brake pads. Then, make the outer face of the brake pads coincident to the caliper’s inner face. You will then want to rotate the pads in the proper orientations and “fix” the pads to prevent accidental rotation. Then, insert the (M5) bolts similarly to step 2. Ensure that your is bolt concentric with both the caliper and the brake pads.
Lastly, we scaled down the sub assembly to 0.6 in order to fit the main assembly.
Step 26: Caliper Brakes (E-drawing)
In this E-drawing, we are depicting a front, right, top, and isometric view. It is noted that the scale for all views (except for isometric) is 1:1. The isometric view is scaled to 1:2. In addition, we are noting the tolerance to be +0.050 mm for each hole in the assembly.
Step 27: Assembly Design Part I
To begin, open up a new assembly on SOLIDWORKS. Then insert the following components:
Housing subassembly, Handle subassembly, Caliper brakes, Lever arm, (2x) Snapping mechanisms, String, brake hook, (4x) M5 50mm Bolts, (6x) M5 70mm Bolts, (6x) M5 80mm Bolts, (14x) M5 Washers, (18x) M5 Nuts, and a B7 Medium threaded rod.
Step 28: Assembly Design Part II
First we will attach the handle assembly to the lever arm by using a coincident mate and a parallel mate to let the handle travel up and down in the z-direction. You can also use a concentric mate to lock the handle in a specific location along the lever arm.
Step 29: Assembly Design Part III
For this second portion, we will use a parallel mate to line up the lever arm with the housing subassembly, then we will use several concentric and coincident mates to attach washers, nuts and 50mm bolts between the housing unit and the lever arm. You can also use screw mates to do this portion instead.
We will also attach two snapping mechanisms to the housing units via M5 70mm, M5 80mm , the remaining washers and some M5 nuts. This is done using concentric and coincident mates but, as stated before, can also be done using screw mates.
Step 30: Assembly Design Part IV
From here we will attach the caliper brakes to the lever arm using a threaded rod and the remaining nuts. Just as before, we will use concentric and coincident mates.
Finally we will attach our string to the assembly. This can be done by using distance mates which can be found under the advanced mate tab.
Step 31: E-Drawing for Assembly
We utilized an exploded view to show our assembly. We simply used the automatic exploded view that SolidWorks offers due to the complexity of the design. In addition, we incorporated the auto balloon function to label each part/sub assembly. We also included a bill of materials.
Step 32: Materials Choice for Manufactured Product
We wanted to design a lever arm that was both strong (high Young’s Modulus) but relatively lightweight (lower density) while remaining in budget. Based on the graph above, aluminum alloys and stainless steel were chosen to use for the lever arm; aluminum alloys have a high Young’s Modulus but lower density compared to other metals, making it suitable for a lightweight lever arm, and steel has a higher Young’s Modulus than aluminum alloys at the cost of a higher density, suitable for parts of the lever arm that face significant stress. Furthermore, both aluminum and stainless steel are weather resistant, making them suitable materials for a product meant to be used in developing countries where they might face wear and tear.
First, a static simulation was run using only aluminum alloy as the material for the lever arm to see if a minimal, lightweight lever arm could withstand the force of a human pushing on the lever. A 130 N normal force, the maximum strength of an average human pushing a lever in the seated position, along the top edge of the lever arm was used to calculate the von Mises strain along the lever.
Because the strain did not exceed the yield strength, 3003-H14 aluminum was deemed an appropriate material for the lever arm; however, 304 2B stainless steel was decided as the material for parts that would face more wear: the gears, pawls, snapping mechanism plates, nuts, bolts, and washers. Based on the calculated volume of the lever through solidworks and the densities of the respective materials, the total mass included 4.1 kg of aluminum alloy and 1.7 kg of stainless steel for a total of 5.8 kg. At $1.90/lb for aluminum and $1.70/lb for stainless steel according to agmetalminer.com, this results in a cost of $23.55 per lever arm, or $47.09 for both lever arms based on raw materials. Steel galvanized wire from Home Depot or any other hardware store can be purchased for the “string” for about $6, and foam pipe insulation as material for the moving handle grip costs about $3, leading to a total cost of about $56.09.
Step 33: Building the Prototype: Tools and Materials
- Drill + battery + drill bits
- Circular file
- Socket wrenchand ratchet heads
- Rubber mallet
- Wood hand saw
- Phillips head driver bit
- Hack saw
- Vice grip/wrenches
- 1.5x2.5x96" Wooden Plank
- 1.25" x 10ft PVC Pipe
- Flat Head Phillips
- #8x1-½ in Wood Screws
- Titebond Wood Glue
- 0.451x23.75x23.75" Wood Sheet
- 5/16" x 12" Wooden Dowels
- 3D printed Gears and Pawls
- M5 Hexbolt Metric 50mm Length
- M5 Hexbolt Metric 80MM Length
- M5 Press Fit Nuts
- M5 Washers
- Compression Spring
Total cost of materials: $53.96
We chose to use wood because it is cheap, durable, and easy to work with using only hand tools. We also decided to 3D print the gears and pawls because of a lack of tools to work with metal. Originally, we were going to use wood for the gears and pawls as well, but we realized that laser cutting those parts could affect their integrity. In addition, we realized that wood would be our best option after realizing the difficulty in working with metals without access to an appropriate workshop.
Step 34: Building the Prototype: Cutting Wood
Cut a 1½ x 2½ in wooden plank to 2ft in length.
Use hand saw to cut a half inch thick sheet of wood into smaller boards of the dimensions given below, to create walls of the housing:
Step 35: Building the Prototype: Putting the Lever and Housing Together
Use two Flat Head Phillips #8x1-½ in wood screws to secure one of the 2x7” boards to the 2ft long wooden plank. The 2 ½ inch edge should be aligned with the long edge of the board, and centered. (For each of the remaining wood screws, drill a hole with a ⅛” drill bit, then use a phillips head driver bit attached to a drill to insert the screw).
Secure the walls of the housing unit perpendicular the largest board (6x7”) by applying wood glue (Titebond) along the edges, then drilling a hole and inserting two wood screws near the corners. Do this with each of the smaller boards, including the one attached to the 2ft plank. Wait 30 mins for the wood to dry before proceeding.
Step 36: Building the Prototype: Gears and Gear Shaft
3D print the gears and pawls from the Solidworks model (two of each). Drill three holes on the 6x7” board at the distances indicated by the Solidworks housing unit model (the rods sticking out). Use a 3/16” drill bit.
Insert M5 50mm threaded bolts into the three holes to serve as axle shafts. Then use M5 press-fit nuts to secure them in place.
For the center gear shaft: First insert six 80mm bolts through the six holes in the first gear (head of bolt in counterbore). Place two M5 washers around the middle bolt on top of the nut, then place the first gear on so the counterbore holes are facing down.
Add three more washers, then place the second gear so that the counterbore holes are facing up (the six bolts threaded through the holes). Add two more washers, and secure with a nut (ideally a locking nut). An alternative to locking nuts is to wrap small elastic polybands around the end of the bolt to prevent the nut from sliding back out of place (We did this in the interest of time and limited materials).
To keep the 6 bolts from sliding down, wrap an elastic around the bolt, then push it down into the counterbore.
Step 37: Building the Prototype: Pawls
For the pawl on the right: thread a nut down the bolt until it is just under the height of the top gear. Wrap an elastic band underneath so the nut doesn’t slide down. Place the pawl on top of the nut, followed by a washer and a nut. Wrap an elastic band around the top to prevent sliding.
For the pawl on the left: Add a washer on top of the base nut, the place the pawl, followed by a washer and a nut. Finish with an elastic band.
For both pawls: Use a ⅜” drill bit to cut a slit into the top of the housing units slightly offset from the pawl. Drill a 1/16” hole into the tapered ends of the pawls. Drill a 1/16” hole into the end of a wooden rod, insert the end of a paper clip so a half inch sticks out, then wrap the remainder of the clip around the dowel. Insert the protruding end of the paperclip into the hole in the pawl, then use an elastic to keep the rod and pawl together.
Cut a spring to the proper length with a hacksaw (ideally a wire cutter) so that it will sit snugly against the top of the pawl and the roof of the housing unit, but not so that the spring is too stiff.
Step 38: Building the Prototype: Directional Levers
On both slits: Drill a hole and insert a wood screw in the wooden dowel slightly above the top of the housing. File a thumb tack down to be little less than a centimeter, and use a mallet to force it into the top of the housing diagonally.
Step 39: Building the Prototype: Snapping Mechanism
Attachment plates: Drill two sets of six M5 holes equally spaced (per the diameters on the model) with a 3/16” drill bit in one of the 4x4” boards.
For the other, drill the outer set of holes, and drill a hole in the center about 1.5” in diameter.
Insert the bolts sticking out of the gears into the the inner set of holes, and secure with nuts and elastics. Insert six 80mm bolts into the outer set of holes on both plates, and secure with nuts and elastics.
Step 40: Building the Prototype: Handle
To create the handle: draw out a circle 1.25” in diameter 2 ft from the center axle with the gears. Then use various size drill bits to remove material from the circle, and file the edges until relatively smooth.
Cut a PVC pipe 7” in length. Use a rubber mallet to force fit the pipe into the large hole to serve as a horizontal handle.
You should end up with a prototype looking like the one above.
Step 41: Building the Prototype: Free Body Diagrams, and Equations
Assume tires do not slip and weight is evenly dispersed across wheelchair. Assume adult male weighing about 70 kg. Assume freedom wheelchair weighs 21.5 lb or 9.75 kg. Assume input force of 65 N (max pushing strength with one hand while seated). Assume rolling coefficient of friction=0.0143, (coefficient of friction between wheelchair and carpet, highest one we could find).
Fn=Normal Force Ff=Force of rolling friction
μ=Rolling coefficient of friction=0.0143
r=Distance from Location of Finput to Point of Rotation=2ft=0.6096m
MA (Mechanical Advantage) = Foutput/Finput
Y-direction: ∑F=0=Wtotal/2 - Fn Fn=(Weight of Man + Chair)/2=(70+9.75 )(9.81)/2=153.3N
We use “sum of the moments” to find out what the output force is, with the help we got from summing the forces in the y-direction: ∑M=(r)(Foutput)-(R)(Ff)=0 Foutput=R(Ff)/r=0.6096(2.192N)/0.3302=4.05N
In our iterative process, we used this information to determine dimensions of the gears and length of the lever arm.
Step 42: Compare Your Files With Ours!
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