THIS PAGE IS OBSOLETE NEW PROJECT HERE!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 relate to the weather here in my region, there were 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


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 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 Exploded View of Incubator

Design Files of Final Project Proposal

Designed Parts

Downloaded Parts


The Egg (Where It All Starts)

  1. In order 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 SolidWorks.

    Egg with caliper for reference

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

    SolidWorks sketch picture tool

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

    Scaling the picture in SolidWorks

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

    Sketching with spline tool in SolidWorks

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

    Revolved Boss/Base in SolidWorks

  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.

    Selecting axis of rotation in SolidWorks

  8. Voila, the virtual egg is made!

    Completed virtual egg in SolidWorks


Bottom Case

Because of the number 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 them.

    Hexagon sketch in SolidWorks

  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.

      Fan space cut in SolidWorks

  3. Screw wizard
    1. In type of Hole, I selected a simple hole as I will later tap the thread.
    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 thread 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.

      Screw wizard in SolidWorks

  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, 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.

      Positioning screw holes in SolidWorks

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

    Resulting screw holes in SolidWorks

  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 initiated, 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.

      Cavity operation in SolidWorks

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

    Part with cavity in SolidWorks

  8. Here you see the cavity.

    Cavity view in SolidWorks


The Crate

  1. The crate was a bit complex to create.

    Crate design in SolidWorks

  2. I started by extruding a cylinder.

    Extruded cylinder in SolidWorks

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

    Half circle cut in SolidWorks

  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 order to create a footprint, I selected the operation subtract.
    4. Last, select the confirmation check mark to finish the combine feature.

      Combine feature in SolidWorks

  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.

      Linear pattern in SolidWorks

  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 by 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.

    Shell feature in SolidWorks

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

    Cutting lower shell in SolidWorks

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

    Complex sketch cut in SolidWorks

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

    Trivial cut feature in SolidWorks

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

    Second linear pattern in SolidWorks

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

    Extruded cut in SolidWorks

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

    Extruded cylinders in SolidWorks

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

    Fillet operation in SolidWorks

  14. The final result of the crate.

    Final crate design in SolidWorks