Parametric Wheelchair Swivel Cupholder

This is a cupholder for wheel chairs that swivels under the arm rest. I took the files from the makers making change website and made them parametric so that it can be adjusted to a certain size that a person wants. It was a little complicated to remake, but if you know how to use fusion 360, you can figure it out. If you just want the files to print it, the STL and fusion files are attached below. To change the width of the cupholder, you need fusion 360. Just go to modify, then parameters and click the cupwidth parameter where it says expression and you can change the width.

To make this or use the files, all you need is the latest version Fusion 360, a 3D printer, software that slices the file so it can be printed, and some filament for the 3D printer. For this I used the Prusa mini printer and Prusa slicer software.

Create a parameter called cupwidth (C) and make it the width you want the cup to be. For this I made it 90mm.

Create a sketch on the xy plane of a circle with the diameter being C

Create another sketch of a rectangle on the xz plane that stretches from the center of your circle sketch to the edge of the circle. make the height C. Make another rectangle that has one edge on that outside line of the big rectangle. Make the height 1/9 of C and the width 1/30 of C. Make the top edge of the rectangle 1/18 of C from the top edge of the larger rectangle.

Now use the revolve feature to revolve your new sketch around the circle sketch. Make sure its function is set to cut so it cuts into it. Select the large part of the rectangle sketch and exclude the smaller rectangle.

Use the shell tool to hollow out this new body. Make the shell thickness 1/15 of C.

Create another sketch on the xz plane that contains two rectangles. Make one of the rectangles 1/3 of C wide and 1/9 of C high. Make the other rectangle 2/9 of C wide and 1/6 of C tall and make the top edge parallel with the top of the cupholder. Make sure that the bottom edges of both rectangle are colinear and the midpoints of those bottom edges coincident on the z axis.

Now extrude each rectangle to opposite sides of the cup holder and set both functions to cut. It doesn't matte how far the extrusions go as long as they cut all the way through the cup holder.

Make another sketch on the yz plane of a rectangle that is centered on the z axis and has a width thats is 1/5 of C and a height that is 5/9 of C. Make the bottom edge 1/10 of C above the xy plane. Then extrude the sketch with function cut out far enough to cut through the cup holder.

Use the fillet tool to curve the edges of the new hole. Set the size to 1/10 of C.

Use circular pattern tool to copy around this hole. Use feature as the object type and select all of the features used to create the hole. Make the quantity 8 but make the compute type adjust so you can select boxes that designate where the holes actually go. Select all of the boxes except the one under the longer slot that you made earlier.

Make another sketch on the yz plane and make a rectangle that is on the outside edge of the cupholder and make it the height of that edge up to the cut that goes all the way around it. The outside edge of the rectangle should be on the outside edge of the cup holder. Make the rectangle 1/30 of C wide. Then make a parabolic curve that starts C/10.3 mm above the top of the rectangle and have the second node go to the the top right node of the rectangle. Then make the node that controls the curve 2/15 of C from the top node of the curve that you first placed. Look at the pictures if your confused. Now finish the sketch and use the revolve tool with the function set to cut to revolve the sketch all the way around. Make sure to select the larger part of the rectangle on the bottom side of the curve to make it so there is a curve edge on the outside.

Use the fillet tool to round off the top edges above the open slot. Make the dimension 1/18 of C.

Create another sketch on the surface of the bottom of the cup holder. First make a circle with a center at the origin with a diameter 7/9 of C. Make a center rectangle with its center at the origin and a length 1/10 of C and a width 1/5 of C. Then make two parallel construction lines that are on the the two shorter sides of the rectangle and stretch out long enough that they go beyond the width of the whole cup holder. Then make two intersecting lines that stretch diagonally from one intersection of the construction lines and the circle previously sketched to the other. Make sure these two lines are intersection at the origin. Now finish the sketch and extrude one side down far enough to cut through the bottom. Make sure you are selection the part that looks like a cone with a flat bottom and you should only be selection one thing for extrusion.

Now use the fillet tool to round off the inside corners of the hole with a dimension of 1/60 of C. Then use the circular pattern tool to copy it around. Select all of the features use to make the hole and set the quantity to 8.

Now select all the edges on the whole cupholder except for the ones you already filleted and fillet them with a dimension of 1/180 of C. The cup holder part is now complete.

Create a new file and remember to make a parameter called cupwidth (C) and make it the same dimension as the one you used for the cupholder part. Create a sketch on the xy plane and sketch a circle with a diameter 96/C and center at the origin. Sketch another circle with a diameter 82/C and center at the origin. Make a line parallel with the y-axis and C/4 from the origin to the left. Make the two endpoints coincident with the outside circle. Make a construction line also parallel to the y-axis but C/3 from the origin to the right. Also make it coincident with the outside circle. On the side with the construction line, make another construction line that is on the x-axis and is 3/9 of C away from the outside of the circle away from it. Make the endpoint of that line the center for a new circle that has a diameter of C/3. Use the offset tool and select the new circle and make the distance C/15 out. Make a construction line that is tangent with the offset circle you just sketch and connects to the point of the construction first construction line in the big circle that is on the same side of the x-axis. To the same thing on the opposite side of the x-axis. On each side make an arc that connects to the end point of the construction line you just made that is on the big circle. Make the other endpoint C/3 from the first and make the arc tangent to the big circle. Once you have done that, on both sides make a sold line all the way across the rest of the that construction line from the end point of the arc to where the construction line connects to the small circle outside. Now complete the sketch and extrude the part shown in the picture above out C/10.3.

Create an offset plane that is parallel to the yz plane and is C/2 from the yz plane. Make a box with the midpoint of the bottom side at the origin. Make the width C/3.07 and the height C/10.3. Finish the sketch and extrude the box towards the origin C/3 or -C/3.

Create a sketch on the xy plane of a circle with the center at the origin and a diameter 7/9 of C. Finish the sketch and extrude it with it set to cut up far enough to cut through your previous extrusion.

Extrude the rest of the first sketch that is outside the big circle or just extrude what is shown in the pictures out C/11.5. Make sure there is a hole in the small circle at the back as shown in the picture.

Create a sketch on the xz plane. Sketch two construction line on the x-axis with one being 21/45 of C and one being 1/2 of C. create another construction line from the endpoint of the smaller line up C/6 and is perpendicular to the x-axis. Make a parabolic curve with the first end point at the end of the longer line and the second endpoint at the end of the perpendicular line you just made. Make the point that determines the curve be 12.8/90 of C above the x-axis. From the top endpoint of the curve make a C/3 long line that is parallel to the z-axis. Draw another line from the endpoint of that line that is C/6 long and is 75 degrees from the previous line you made. Draw another line from the endpoint of that line that goes down to the x-axis but makes a 75 degree angle with the x-axis. draw a line along the x-axis from the endpoint of the previous line you made to the bottom endpoint of the curve to close the shape. Finish the sketch and on each face extrude out 3/180 of C to make the body a total of 3/90 of C thick.

Make another offset plane that is parallel to the yz axis that is 26/45 of C from the origin. Create a sketch on that offset plane. Draw a line with an endpoint one edge of the body that you made in the previous sketch that is C/9 down from the very top of that body and make the other endpoint be on the face of the large body below as shown in the pictures. Make the angle that the line makes with the face of the larger body be 60 degrees. Do the same thing on the other side of the z-axis. Finish the sketch and extrude both sketches C/30 towards the origin.

Use the fillet tool and select all of the edges except for the ones highlighted above and make the dimension C/180. For the edges in blue make the dimension C/50 and for the edges in red make the dimension C/25. The holder is now complete.

Create a new file and remember to make a parameter called cupwidth (C) and make it the same dimension as the one you used for the cupholder part. Create a sketch on the xy plane of a circle with a diameter 6/9 of C and its center at the origin. Finish the sketch.

Make an offset plane parallel to the xy plane that is C/11 above the xy plane. Create a sketch of a circle on the offset plane with a diameter 7/9 of C. Sketch another circle with a diameter of C/3.2. Make both of the centers of these circles at the origin. Finish the sketch and extrude the smaller circle up C/10.

Select the loft tool and for profiles select the outside edge of the circle on the xy plane and the outside edge of the large circle on the offset plane and then finish the loft.

Create another sketch on the face of the small cylinder on top of the body. Select the outside circle with the offset tool and create an offset that goes in C/18 or has a dimension of -C/18. Finish the sketch and extrude the small circle up C/18.

Create another sketch and the top face of the smallest cylinder at the top of the body and sketch a circle that has a width of C/3.2 and should line up with the circle below the sketch. Draw two intersecting lines that are coincident with the outside edges of the circle and are the length of the diameter of it. They should be intersecting at the origin make an angle between the two lines 100 degrees and then finish the sketch. Extrude the small inside circle and the two small sections of the outside circle that the lines create or that are 100 degrees. Extrude that up C/18.5.

Use the fillet tool and select all of the edges of the entire body and make the dimension C/180. The plug is now complete.

Create a new file and remember to make a parameter called cupwidth (C) and make it the same dimension as the one you used for the cupholder part. Create a sketch on the xy plane of a circle with a diameter of C/3 and its center at the origin. Use the offset tool to create two offsets from the circle with one going out C/15 and the other going in C/9.2 or the dimension -C/9.2. Sketch two lines that are both diameters of the first circle and intersect at the origin. Make the angle between them 99 degrees. Extrude the part between the inner offset and the initial circle that the two lines create and is the larger section or the section that is 99 degrees. Extrude that up C/18.5. Then extrude the section between the outer offset and the initial circle up C/7.

Create a sketch on the faces of the shorter sections of the body and copy the same C/3 circle as before and the same -C/9.2 inner off set as before so the line up with the edges of the body. Make a line that is the diameter of the C/3 circle which passes through the origin. Make it 8 degrees from the one of the lines you made in the previous sketch and make it so it creates a little section on both of the small circular bodies that you can extrude. Look at the pictures for clarification. Extrude both of those small sections up C/18.

Create another Parameter that will dictate the width of the bases so that the width can be fitted to the width of a the bar the cup holder will go on with out changing the size of the whole cup holder. Call the parameter basewidth (B) and for now make it the same width as C but you can change it later to fit the wheel chair better.

Create a sketch on the top face of the body and sketch a center rectangle that is B long and C/2 wide. Make another rectangle on the right side of the y-axis that has its top edges along the longer side of the large rectangle with its length being C/9. Make another rectangle that is C/25 long and the midpoints of its top edges on the left edge of the larger rectangle you just made. Make the top edges of the small rectangle equidistant from the top edges of the large rectangle and make the width of the small rectangle C/3. Make the right edge of the small rectangle C/30 away from the right edge of the first large rectangle you made to shift the two rectangle to the right edge of it. Then mirror the two inner rectangles across the y-axis to the left side of the first large rectangle. Finish the sketch. First extrude the parts of the two large inner rectangles that the small inner rectangles do not intersect up C/15. Extrude the rest of the overall rectangle not including the small inner rectangle down C/30 or with a dimension -C/30.

Copy and paste the entire body and move the new body away so that they are separate. Then use the extrude tool to remove the large inner rectangle extrusion by selecting those two top faces and extruding them down C/15 or a dimension of -C/15.Now you have a flat version for flatter surfaces.

Use the fillet tool and select all of the edges of the entire body and make the dimension C/180. The bases are now complete.

On the same file, create an offset plane parallel to the xy plane that goes up C/9. Create a sketch on that plane with a circle that has a diameter of C/3.1 and its center at the origin. Make an offset from the circle that goes in C/35 or has a dimension of -C/35. Create two diameter lines on the outer circle like how you have done before so that they intersect at the origin. Make so that they are both C/300 away from the edge of the inner sections of the main body like how it is it the picture above. Finish the sketch.

Extrude the two smaller sections in between the offset and the outer circle the the lines created down C/9.5 or a dimension of -C/9.5. Extrude the whole circle up C/30. Move the new body away from the Base so that it is not intersecting.

Use the fillet tool and select all of the edges of the entire body and make the dimension C/180. The top is now complete.

Now you can upload the STL files to Prusaslicer or whatever software you are using and 3D print the cupholder. Look at the assembly guide at the top of the photos attached here to figure out how to put together.