THIS PAGE IS OBSOLETE NEW PROJECT HERE!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 farming needs.

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

Chickens!

For reasons I believe relates to weather here in my region, there was no available chicks to be bought in the local farms cooperative, so I decided I would make a Chicken incubator.

Design Files of my new proposition

Video render and link of my possible final project proposal page

Egg Incubator

Details of my Final Project.

Solid works has been my software of choice for the last years when it comes to mechanical design. I am very happy with it as its powerful and allow quite complex assemblies at the same time been intuitive enough for me to learn by using it.

Exploded View of Incubator

    Design files of final project proposal

    Designed Parts

  1. Egg
  2. Case (top)
  3. Case (bottom)
  4. Egg Crate
  5. Heat Element
  6. Water

    7. Downloaded Parts

  7. Fan Designed by Xgentec Jason at Grabcad
  8. Servo Motor Designed by Akshaya Simhaat Grabcad
  9. Ball Bearing Designed by Hendricks at Grabcad
  10. Oled Display Designed by thmjpr at Grabcad
  11. Humidity Sensor Designed by Nonthanut Hoku at Grabcad

The egg (where it all starts)

  1. In other to design my final project I started with designing an egg.
  2. I took a picture of a real egg with the caliper for reference later in solid works

  3. To use the feature start a new skecth the in the menu go to: Tools > Sketch Tools > Sketch Picture.

  4. After inserting the picture scale it using the caliper reference as well as the blue ruler provided by Solidworks.

  5. With the picture calibrated to scale its time to sketch around. For this I used spline tool and closed the spline with a construction line

  6. Leave the Sketch and Click on Revolved Boss/Base

  7. 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.

  8. Voila the virtual egg is made!

Bottom Case

Because of the amount of steps I will only detail the most important ones specifying the type of operation in the beginning and then some of the steps to accomplish it.

  1. I started by sketching 2 hexagons and extruding it.

  2. Converting a contour of another object in an assembly:
    1. With the fan already mated with 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

  3. Screw wizard
    1. In type of Hole, I selected a simple hole as I will later tap the tread.
    2. In the standard, I selected ISO as it contains metric screws.
    3. In type of drill, I selected tap drill as this will give the right clearance to use a manual tap to open a tread later.
    4. Here I selected the size of the screw M3
    5. Next I clicked in position to determine where the holes will be located.

  4. Position of screw holes:
    1. The point sketch is normally selected already unless you had to create construction lines or other operations.
    2. Next with the I centered each point on the locations where the fan will receive the screws.
      3. last confirm and close the operation and the result will be holes created in the surface previously selected.

  5. Here is the result of the previous operation the holes in place.

  6. Cavity, this operation is useful as it will save time designing many features that in this example will be simply inherited from the selected object or body:
    1. Simply start by either searching in the search menu for "cavity" or finding it on the "insert" "features" menu. After the feature is initiate, I selected the part I wanted to inherit the features creating a kind of negative stamp in my part.
    2. then simply confirm the operation

  7. Here you see the part with the caity already created.

  8. Here you see the cavity.

The crate

  1. The crate was a bit complex to create.

  2. I started by extruding a cylinder

  3. Next I cut it in half by sketching a half circle on one of its faces.

  4. This time I used the combine feature instead of cavity.
    1. The main body should be already selected by default
    2. Next I selected the part I wanted to combine
    3. In other to create a foot print I selected the operation subtract
    4. last select the confirmation check mark to finish the combine feature.

  5. Linear Pattern is a feature used to replicate in various directions a feature so it saves time instead of designing the pattern feature again and again:
    1. I started by selecting the pattern.
    2. then I selected the distance between the patterns
    3. then I specified it to replicate it 3 times.
    4. next I confirm

  6. 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 specifying the thickness, in my case 3mm and I did not have to select the body as it was already selected before initiating the feature

  7. Now in other to expose the previous feature I cut the lower shell by sketching around the lower shell of the body.

  8. This was a simples cut feature with a complex sketch. The sketch was created by off setting inwards the outer contour, drawing lines towards the center and last trimming all the lines in other to form closed perimeters that were used to cut the shape.

  9. The cut feature is trivial and was done simply selecting the previous sketch and cutting it through all.

  10. This was again a linear pattern done in the same manner as the previous one.

  11. I then Extruded cut the rest of the wall off the once shell of the half cylinder.

  12. Last I extruded cylinders in between each basket to work as a shaft.

  13. Fillet was used everywhere in this part hgere I exemplify the shaft being reinforced with the fillet operation.

  14. The final result of the crate