Final Project CAD

DESIGNING THE EGG:

Since I had to start somewhere, I decided to start with the egg itself. Its size would be my greatest constraint, considering that I had to fit all of my electronics inside it. 

Google—and a call home to ask my mom to measure some eggs from her fridge—informed me that large chicken eggs average about 60mm long and 44mm in diameter. I took the liberty of adding a little bit of wiggle room for my electronics, figuring I could always scale downing my second spiral if I achieved success at this size. So my first egg ended up being more of a “jumbo” egg (or duck egg!), though I scaled it down later. 

To design this in Fusion, I first used construction lines to map out the maximum height of my egg: 75mm. Then I inserted an image of an egg from Google into my sketch as a canvas. (This was the first time I've used the "canvas" feature, but it won't be the last. It's super handy! It basically just drops an image into the background of your design so that you can use it as a template for sketches, etc.)

I scaled the image until it was the same height as my construction lines, making sure to keep the image centered over the origin since I knew I'd want to reflect things across centerpoints later. Then I used the "spline" function to trace along the right side of the egg's perimeter. Finally, I drew a straight line along the y-axis (at the origin) from the bottom of the egg to the top. My finished sketch was of one full half of the egg.

Then, because I am overzealous about parameterization (thanks to Alfonso!), I wanted to parameterize my egg. 

Although there’s no straightforward way to parameterize splines, I found a workaround: I used the “sketch dimension” tool to determine the distances between each of my spline points and several fixed points on the egg. (I used the center line and each pole for reference.) Now, instead of dragging the spline points to change the egg’s size, I could enter new values into the dimension boxes.

I could theoretically have made each of these dimensions a parameter and enter the values that the sketch dimension tool had initially yielded. This would preserve my current sizing while building in quick-adjustable parameterization. However, there were six (6) diameter measurements and seven (7) vertical distances. That was a lot, and I’d have to assign a name to each one that would make sense later. Or perhaps draw a reference diagram and just assign each one a shorthand letter or some such. Since I can realistically just edit the dimensions in the sketch easily enough, I decided to stick with that. 

Once I had my half-egg drawn, I simply used the “revolve” function to revolve it 360 degrees around its z-axis. This produced a three-dimensional egg.

DESIGNING THE MOLD & REGISTERS

My next step was to create the frame for my mold. I followed the same steps here as outlined in week #8. 

First, I created a bounding box slightly larger than my egg and extruded it down below its bottom edge. Then used combine -> cut to carve an egg-shaped hole in the box, making sure I checked the box to keep the tool for future use. (In this case, the tool was the 3D egg form).  

Then I added registers. I knew I wanted to include both hemispherical and step registers since the combination had worked well for me during modeling and casting week. 

To make the hemispherical set, I created a new sketch on the top face of my mold (the surface with the egg carved out of it). Then I drew construction lines connecting opposite corners to create an X in the mold's center. I sketched a small circle near one corner, and used the mirror/reflect function to rotate it into three dimensions to create a sphere, and used the reflect tool to replicate this in my other three corners. Now I had spheres in all four corners of my mold, which I could use to create my registers.

To make positive registers, I selected the two spheres in diagonally opposite corners (upper left and lower right) and used combine -> join to fuse them to the mold's frame. To create their negative counterparts, I selected the opposite spheres and used combine -> cut. 

At this point, I made a copy of my mold, translating this just far enough to the right that it sat nicely beside the original. Now I had two mold halves, laid out side by side.

To create my step registers—which I angled at ~45 degrees to make the mold easier to take apart—I created another new sketch on the surface face of my original mold. I drew a new bounding box within this sketch, offset slightly inside of the original mold frame. Then I extruded this upward slightly, and used the chamfer tool to slice its inner edges down. This gave me a gently sloping frame. 

Before joining this new "step up" with my left mold frame, I duplicated it and translated it the same distance over as my original mold. I then joined the original mold and "step up" frame into one piece (a new component). This was the left half of my mold. To finish the right half, I selected the duplicate step and reflected it over the surface plane, creating a new body. Then I merged this new body (a "step down" frame) with the right mold half, creating a new component once again.

EGG STAND: 2D DESIGN & LASER CUTTING

As a last step, I needed to tackle the 2D design and subtractive fabrication portions of the final assignment to make a nice display for my egg. 

(I'd originally been planning to mill machinable wax for my subtractive process, but ended up 3D printing my mold instead since the oomoo would have reacted poorly with my silicone.)

I used Fusion 360 to design a flat-pack, press-fit wooden stand for my egg. 

To ensure a perfect fit, I first copied over my original egg sketch and body from my mold design. Then I projected the egg's silhouette onto a new sketch and traced splines around this until I was happy with their shape. These would be my stand's legs. 

Inspired by the bubbles in my cast, I added circular design elements. Then I extruded the silhouette to the width of my material (3mm plywood). Now that I had a finished leg, I used the circular pattern function to create four more legs (five in total) equally spaced around my egg.

Next, I moved down to my bottom plane and constructed a new sketch: a center-point circle at the origin. I extruded this my material width, translated it up the z-axis until it was approximately where I wanted my stand's platform to be, and press-pulled it until it was a pleasing size. I then repeated this process with a second circle slightly farther down, below the bottom of my egg.

Now that I had all of my parts created in three dimensions, I needed to add slots. I revisted the sketch for my leg and added slots that were half the depth ultimately wanted (since they'd be scissor-fit with the circular platforms, which would share the slot depth).

Then I used my slot-equipped leg as a tool to "cut" into each of the circular platforms.

As a last step, I made copies of my pieces and rotated those copies to be parallel to the bottom plane. Then I created a new sketch, and projected them onto it.

Finally, I exported the projections as a .dxf file, put them onto a USB, and used the EECS laser cutter to cut them out of 3mm plywood

I broke one of my smallest circles when assembling, but thankfully had made some extras. I'm pleased with the finished product