Training Part 2.1 - CAD Arduino Holder

Here is a link to download the PDF drawing

https://drive.google.com/file/d/1IykuGNM...

NOTE* THIS DOZUKI CAN BE COMPLETED MANY WAYS

1) If you are already familiar with Fusion 360, then use the drawing to complete the part

2) If you are competent, but still not sure about some feature, just skip to the Step with the feature you need help understanding

3) If you are not sure about how to start, follow this dozuki through its entirety, and it will walk you through start to finish

This step is not necessary and can be skipped

When we begin drawing a CAD file, it is a good practice to observe the part

From here we began by creating 2D shapes.

We then use these 2D shapes to create 3D objects in space.

The picture is a highly detailed flow chart of the engineering design process.

Start the program Fusion 360

Select your name on the top right of the screen

Make sure the "IFL - Team" is selected

Select "IFL - Team"

If "IFL - Team" is not available, contact either David Kriesberg or Kenny Davis Jr to be added

Began by clicking the file button (circled in orange), and select "New Design"

This can also be accomplished with Cntl+N

As with every CAD file, we will begin by creating the most basic shape

Looking at the CAD drawing, we see that a RECTANGLE is the most basic shape, so keeping that in mind, we will start a new sketch

Remember for every CAD model, we begin in 2D, and then move to 3D. This is why we are starting with a rectangle, and then we will "bring it into 3D"

Click the "Create Sketch" button (red circle), then, select the XY or "top" plane (red rectangle)

Maneuver the view to a plan view, this can be accomplished by selecting "Top" on the view cube

In the "sketch" tab, click the drop down menu named "create," and click "rectangle" and then "2-point rectangle"

First click in the origin (pink circle), then type in the dimensions (pink rectangles) you found on the drawing (3.94 x 5.42) and hit enter

Type in one dimension number, then TABing will take you to he other number

Now that we have our rectangle in 2D, we will simply extrude it out

Begin by going to the "solid" tab, and dropping down the "create" button, and select extrude from the option

This will then prompt an "extrusion command center" as shown by the orange square, there isn't much to do here except type in our thickness and enter

For any questions on what any of the options mean, ask any IFL staffers or slack Kenny Davis Jr

When finished, it should look like the pink circle

We will begin by creating a square on the top, and extrude cutting through

Begin by selecting the top surface, and then selecting "create new sketch (red rectangle)

Change the view to the "top" view, an draw a rectangle (look at step 4, the green sub-bullet) with the dimensions from the drawing (2.27 x 3.38)

Location can be approximate

Next, we are going to define where it is with reference to the outer body

Select the dimension tool (green square) by going to "create" and the clicking "dimension all the way at the bottom

Continue on to part 2

Dimension from the outer edge to the rectangle both .28" (red squares)

Then, go to the "solids" and select "extrude"

For the body we are extruding, be sure sure to select the inside of the rectangle we drew in step 6

Now input .12 in but make sure that the operation is set to "cut" (pink square), and hit enter to see the new cut feature

Let's first begin by selecting our top surface again and drawing 1 rectangle (2.56 x 3.23)(red rectangle)

Now let's dimension off our rectangle, select the dimension tool, and offset .36X and -.21Y (orange rectangle)

Finally, in order to create a uniform wall thickness, let us select our offset tool by going "Modify" in the "Sketch" tab, from here drop down the menu and select "Offset"

Now with the offset tool selected, we can select the rectangle we just drew, and type our thickness of -.2"

The reason the value is negative is simply because the offset would go on the outside if it were positive, if you are unsure what I mean, type in .2" and see what happens

With the outline of the arduino wall, we can now extrude, go ahead and select extrude, then extrude out the wall region we just offset by .24"

When finished, the part should now look like the last figure

Begin by creating a sketch on the right facing wall we just created, and go into plan view

Next create 2 point rectangle, and make sure to select the top line first as shown by the arrow, and input the dimensions .55x and .1z

Selecting the top line will create a relationship where the point of the rectangle is "hooked" to the top, and this is exactly what we need

Dimension .57" from the outside of the wall

Now simply select extrude, and cut away -.2" (the thickness of the wall)

Remember cutting away requires a negative distance

Begin by selecting the surface where the Arduino goes, then start a new drawing.

Draw the sketch given in the second photo. All of the distances and lengths are given.

Be sure not to leave any blue lines, which means the sketch has undefined properties.

When finished, simply select the four circles and "extrude" shown by the green circles. Make is ".12" tall.

Begin by selecting the surface in blue, as shown by the red rectangle.

Create a new sketch, and draw 3 rectangles as shown in the second picture. All dimensions are given.

Finally, extrude down to the bottom of the breadboard surface. This will cut down to the surface requested, as shown by the red cut away.

Again chose the middle surface as shown by the red rectangle.

Use all the dimensions as given by the second picture.

Extrude down to the bottom surface.

All of the steps are a repeat of the previous step.

Begin with the chamfers on the Arduino older. Select all the corners in the red circle and select "chamfer."

The chamfer should be .09"

Next, select the "radius" tool and select the inside corners of all 5 rectangles we drew for the breadboard cutout.

The radius should be .0625"

Lastly, select all four corners of the part, shown in the green circles.

Radius to .2"

Began by selecting the middle surface again. Create a sketch off here.

Draw 4 circles at .15" in diameter, and .2" off the walls, as shown by the orange circles.

If more advanced, draw one circle and mirror it over, but this is not necessary.

Lastly, extrude all 4 circles "through all."

Here are 3 different views of what the finished part should look like.