Project Update - Fab Academy 2020

THIS PAGE IS OBSOLETE, NEW PROJECT HERE!

Final Project Concept Update and Design Files

During week 2, I decided to change my project to one that is more in sync with the farm's needs.

I asked myself what I needed right now for the farm that I couldn't just obtain.

Chickens!

For reasons I believe are related to the weather here in my region, there were no chicks available to buy at the local farmers' cooperative, so I decided I would make a chicken incubator.

Design Files of My New Proposal

Incubator files on the Fab Academy GitLab

SolidWorks design view of the incubator

Video Render and Link of My Possible Final Project Proposal Page

Egg Incubator

Details of My Final Project

SolidWorks has been my software of choice for the last few years when it comes to mechanical design. I am very happy with it, as it's powerful and allows quite complex assemblies while being intuitive enough for me to learn by using it.

Exploded View of the Incubator

Design Files of the Final Project Proposal

Incubator SolidWorks source files on the Fab Academy GitLab

Designed Parts

Egg
Case (top)
Case (bottom)
Egg Crate
Heat Element
Water

Downloaded Parts

Fan designed by Xgentec Jason on GrabCAD
Servo Motor designed by Akshaya Simha on GrabCAD
Ball Bearing designed by Hendricks on GrabCAD
OLED Display designed by thmjpr on GrabCAD
Humidity Sensor designed by Nonthanut Hoku on GrabCAD

The Egg (Where It All Starts)

In order to design my final project, I started by designing an egg.
I took a picture of a real egg with the caliper, for reference later in SolidWorks.
To use this feature, start a new sketch, then in the menu go to: Tools > Sketch Tools > Sketch Picture.
After inserting the picture, scale it using the caliper as a reference, as well as the blue ruler provided by SolidWorks.
With the picture calibrated to scale, it's time to sketch around it. For this, I used the spline tool and closed the spline with a construction line.
Exit the sketch and click on Revolved Boss/Base.
If the axis of rotation is not selected automatically, select the line that is in the center of the future egg. Press the green check mark.
Voilà, the virtual egg is made!

Bottom Case

Because of the number of steps, I will only detail the most important ones, naming the type of operation at the beginning and then some of the steps to accomplish it.

I started by sketching 2 hexagons and extruding them.
Converting a contour of another object in an assembly:
1. With the fan already mated to the sides of the case, I selected the outside contour of the fan and converted it, creating a sketch.
2. Next, I cut the space for the fan.
Hole Wizard:
1. In the hole type, I selected a simple hole, as I will tap the thread later.
2. In the standard, I selected ISO, as it contains the metric screws.
3. In the type of drill, I selected tap drill, as this gives the right hole size to open a thread later with a manual tap.
4. Here I selected the screw size, M3.
5. Next, I clicked on Positions to determine where the holes will be located.
Position of the screw holes:
1. The sketch point is normally already selected, unless you had to create construction lines or other operations.
2. Next, I centered each point on the locations where the fan will receive the screws. Last, confirm and close the operation, and the result will be holes created in the surface previously selected.
Here is the result of the previous operation, the holes in place.
Cavity: this operation is useful as it saves time designing many features that, in this example, are simply inherited from the selected object or body:
1. Simply start by either searching for "cavity" in the search menu or finding it in the "Insert" > "Features" menu. After the feature is started, I selected the part I wanted to inherit the features from, creating a kind of negative stamp in my part.
2. Then simply confirm the operation.
Here you see the part with the cavity already created.
Here you see the cavity.

The Crate

The crate was a bit complex to create.
I started by extruding a cylinder.
Next, I cut it in half by sketching a half circle on one of its faces.
This time I used the Combine feature instead of Cavity.
1. The main body should already be selected by default.
2. Next, I selected the part I wanted to combine.
3. In order to create a footprint, I selected the Subtract operation.
4. Last, click the confirmation check mark to finish the Combine feature.
Linear Pattern is a feature used to replicate a feature in various directions, so it saves time instead of designing the same feature again and again:
1. I started by selecting the feature to pattern.
2. Then I selected the distance between the copies.
3. Then I set it to replicate 3 times.
4. Next, I confirmed.
Here I used the Shell feature, as I wanted to keep the contours but I wanted the interior to become empty. This was done simply by specifying the thickness, in my case 3 mm, and I did not have to select the body, as it was already selected before starting the feature.
Now, in order to expose the previous feature, I cut the lower shell by sketching around the lower shell of the body.
This was a simple cut feature with a complex sketch. The sketch was created by offsetting the outer contour inwards, drawing lines towards the center, and finally trimming all the lines in order to form closed perimeters that were used to cut the shape.
The cut feature is trivial and was done simply by selecting the previous sketch and cutting it Through All.
This was again a linear pattern, done in the same way as the previous one.
I then used an extruded cut to remove the rest of the wall from what was once the shell of the half cylinder.
Last, I extruded cylinders in between each basket to work as a shaft.
Fillet was used everywhere in this part. Here, as an example, the shaft being reinforced with the fillet operation.
The final result of the crate.