General steps required:

Switching to the Manufacture workspace in fusion
Creating a new manufacturing setup
Creating and configuring a new toolpath for each cut (this guide covers 2D contour and 2D pocket operations )
Exporting .gcode files for use in Bantam software

General considerations:

It’s easier to generate toolpaths if you create your models in the Z up orientation
You will need to create a new setup for each part that needs to be cut from a different piece of stock material
It’s important to download and install the Bantam Tools Library for Fusion 360. Follow this link for the most updated version
Currently the maximum pass depth that we use is 0.003 inches (or 0.0762 mm)

For this guide we’ll use the following 3D model, which is designed to be cut out of ¼” aluminum stock.

This part will require a 2D contour operation for the perimeter of the shape and a 2D pocket operation for the inside pocket.

Make sure you are in the Milling panel
Under the Setup dropdown menu, click the New Setup button
In the SETUP:SETUP1 panel that is now open, make sure you are in the Setup tab (the first one)
Under Machine, select Autodesk Generic 3-axis with the Y axis on the table and XZ axis on the head

If you have more than one body in your file, use the selection tool under Model to select the body you want to generate a toolpath for.
Move to the Stock tab (second from the left)
Under Stock, select Relative Size as the Mode
Add some offset to Stock Side Offset (this is useful for visualizing contour cuts and tabs)
Leave all other offsets at 0
Click OK to finish creating the setup

In the 2D CONTOUR panel, in the Tool tab, select the appropriate tool from the Bantam Tools Fusion 360 Tool Library. For this example, we are using a 1/16” flat end bit.

In the Geometry tab, under Contour Selection, select the bottom contour of the profile you need to cut
Check the Tabs box
Set the Tab Width and Tab Height (1.5 by .4 mm works for aluminum)
Set the Tab Positioning to At Points
Click the positions at which you want tabs along the selected contour

Bottom contour selected and tabs positioned

In the Passes tab, check the Multiple Depths box
Change the Maximum Roughing Stepdown and Finishing Stepdown to 0.0762 mm (3/1000”)

Pass depth configuration

Hit OK
In the Milling tab, click ACTIONS and select Simulate from the drop down menu
Run the simulation and make sure everything looks OK (passes and tabs)

Contour simulations with passes (blue) and tabs

In the 2D POCKET panel, in the Tool tab, select the appropriate tool from the Bantam Tools Fusion 360 Tool Library. For this example, we are using a 1/16” flat end bit.
In the Geometry tab, under Pocket Selections, select the bottom bottom surface of the pocket you need to cut

Pocket selection

In the Passes tab, under Maximum Stepover, input half the diameter of the bit (or less). In this example, we are using a 1/16” bit, which is 1.5875 mm, so we are using a stepover of 0.75mm
Check the Multiple Depths box
Change the Maximum Roughing Stepdown and Finishing Stepdown to 0.0762 mm (3/1000”)
Uncheck the Stock to leave box
Hit OK
In the Milling tab, click ACTIONS and select Simulate from the drop down menu
Run the simulation and make sure everything looks OK (passes and perimeter of the pocket)

Select one of the toolpaths in the Project Browser
In the Milling tab, click ACTIONS and select Post Process from the drop down menu
Under Post, click the drop down menu and select Choose from library
Enter “Bantam” in the search box
Click the Bantam Tools post and click Select
Input a File name and select the Output folder
Click Post
You will find a .gcode file in the specified location
Repeat this process for all your toolpaths
The .gcode files will be ready to be loaded into the Bantam Software to perform the cuts

The finished piece