Begin by creating a sketch in the Fusion 360 Design workspace. Select a construction plane to place geometry. The Top View is a good starting point but any orientation will work.
Place an eight inch circle in the center of your grid.
Draw a one inch circle at X0.0 Y3.2 position on the sketch grid. Use the mouse cursor to reference from X0. On your keyboard type “d” to activate the dimension tool. Dimension the vertical distance 3.2″ from the origin.
On the Sketch Toolbar; click the drop down arrow, then click on Circular Pattern.
- Click on the Object Select button.
- Select the 1″ circle.
- Click on the Center Point Selection button.
- Select the 8″ circle to utilize the center point. This will be the center point that the circular pattern will revolve around.
In the Quantity box; input a quantity of 8. This will create an eight hole bolt circle.
On your keyboard, type “E” for extrude. Select inside the 8″ circle to extrude the drawing profile. Enter 1″ in the Distance input and hit enter or OK.
Congradulations! You just created your first solid body.
Create a sketch on the face of the solid body.
Draw a 1/2″ circle in the second quadrant.
Using the dimension tool; constrain the 1/2′ circle to the X1.5 Y1.25 position:
- Vertical = 1.25
- Hoizontal = 1.5
- Select the “Create” dropdown On the “Sketch” toolbar.
- Select the Rectangular Pattern tool.
Select the circle as the “Object.”
Input the direction and distance parameter below.
- Direction – Right
- Quantity – 5
- Distance 2.75
- Direction Type – One Direction
Vertical Pattern Direction
Pull the blue arrow downward to copy and translate the pattern in the vertical direction.
- Quantity: 2
- Distance: -.875
- Draw a horizontal line that begins at X0.0 Y0.0 center of the model.
- Select the line and transform it to a “Construction” line by typing “x” on your keyboard.
Activate the “Mirror” function on the 2D Sketch toolbar.
- Object: Select the group of circles
- Mirror Line: Horizontal Construction line
Verify the Mirror preview looks correct.