Computer Aided Machining (CAM) is the process of translating a CAD model into machine instructions that a CNC can execute. This module introduces key CAM concepts, including setting up toolpaths, selecting tools, and generating the G-code needed for CNC operation.

Basic CAM Concepts

• Toolpaths: Toolpaths determine the movement of the cutting tool relative to the workpiece. Strategies such as contour cutting, pocketing, and drilling are used depending on the desired outcome.
• Operations: CAM operations are the specific tasks needed to machine the part, including profiling edges, cutting pockets, or drilling holes. Each operation requires setting parameters such as cutting depth, speed, and feed rate.
• Tool Selection: Tools vary by size, shape, and material, with each type optimized for specific operations and workpiece materials. Tool selection can be limited by the collet capacity (ER11, or ≤7mm), spindle torque and speed and material selection. Generally, select a right-size tool for the job and consider your operation order to minimise changes (due to the lack of a toolchanger).
• Feeds and Speeds: Feeds and speeds refer to the cutting parameters, specifically the feed rate (how fast the tool moves across the surface of the material) and the spindle speed (how fast the tool rotates). Selecting the appropriate feeds and speeds is crucial for achieving optimal cutting performance, prolonging tool life, and ensuring a quality finish. Incorrect settings can lead to tool wear, poor surface quality, or even tool breakage. Read more about feeds and speeds.
• Chips: In CNC machining, heat is a major issue to be managed. The tool spins at very high speeds, and excess heat dulls cutters, burns workpieces and increases deflection and tool breakage. The ideal form is the chip, a small piece of material relative to the tool’s cutting edge, which due to its mass and way it’s created holds the heat generated and moves it away from the cutter and the workpiece.
• Together, Feeds and Speeds and Chipmaking are the way that heat is managed in machining. A well formed chip is large enough to carry away the heat generated; it will only be formed if the physics of how the cutter moves across the work surface are coordinated.

Setup Fusion 360 for CAM at VHS

Certain machine-specific settings are contained in files which must be imported in Fusion 360. Install these files before beginning any CAM work, as they contain necessary information for Fusion 360 to be able to correctly format and output data to the CNC.

• The Post File: The 'Post' file, or post-processor file, translates tool paths generated by CAD/CAM software into a specific format that the CNC machine can understand and execute. To install this file:
  • Download the post file and decompress it.
  • In Fusion 360, go to the 'Manufacture' workspace, then on the toolbar's 'Manage' section, select 'Post Library'; a Post Library window will open.
  • On the left, select 'Local' under 'My posts' as the target install location, then click the import icon in the centre pane of the window. Select the post file from your computer. You should see an entry in the centre pane with the new post file.
  • You will use this file in the next section.
• The Machine Library: Hold definitions of the target machine's kinematics, geometry and configuration, as well as the post file to use and where to output files for manufacturing. To create the machine definition for VHS Dustie:
  • In Fusion 360, go to the 'Manufacture' workspace, then on the toolbar's 'Manage' section, select 'Machine Library'; a Machine Library window will open.
  • Open the 'Fusion Library' section (left column) and select 'Autodesk' from the list of manufacturers.
  • In the list of machines, select 'Autodesk Generic 3-axis Router', specifically the one with YXZ kinematics to match the actual machine.
  • Copy the machine (using the controls at the top of the window or the right mouse button), navigate to My Machines > Local (left column), and paste the machine into your local library.
  • Right click on the machine in your local library and select 'Change the selected post'; then select the VHS Dustie post file from your local library.
• The Tool Library: Hold information about both the tools (end mills) and the toolholders (the collet and spindle) used on the CNC machine. Like post files, it is also found in the 'Manufacture' workspace's 'Manage' section. As Fusion 360 is used in many contexts, we will focus on 'Milling Tools' only, for simplicity. The library has the following functions:
  • Storing a library of your personal tools (left column)
  • Offering a catalogue of pre-definied name-brand (Vendor) and generic (Fusion Library) tools (left column)
  • Creating, copying and removing tool definitions in your library
  • Filtering the list (right column)
• For your training, either enter the tools you have purchased in this utility, or discuss with your instructor the tooling which will be provided. To import tool definitions, open the provided csv file in a text editor, copy the entire contents, then navigate to Fusion 360's Local Library (left column) and use the 'paste' function in the tool list (centre).
  • Training Tools (Martin Ciastko)

<WRAP center round info 100%> </WRAP> <WRAP center round download 60%>

• VHS Dustie Post File
• Training Tools (Martin Ciastko)

</WRAP>

Workflow in Fusion 360

In Fusion 360, CAM is integrated directly, enabling a smooth transition from CAD to CAM. CAM tools are found by changing the Workspace to Manufacture. The typical workflow involves:

• Define Machine and Tools: Define machine parameters, including how the machine moves and specifying a post file that prepares toolpaths for compatibility with the specific CNC. Select the appropriate cutting tools from the tool library or define new ones if necessary. This is typically performed once for the machine and updated when new tools are added.
• Create a ‘Setup’: The setup defines the machine, workpiece dimensions, reference point and the coordinate system. There can be multiple setups, for example when reorienting the workpiece.
• Toolpath Creation: Once you have a setup defined, select the desired operations and generate toolpaths. Feeds and speeds are set during this step. This usually is a two-step process, with operations classed as either:
  • Roughing: Efficiently cut away large amounts of material using operations designed for fast removal of large amounts of material, at the expense of quality. (e.g. 2D Adaptive Clearing, 3D Adaptive Clearing, Face).
  • Finishing: Use slower techniques to remove remaining material, with movements tuned to give high-quality finishes. (e.g. Contour, Parallel)
• Simulation: Use the simulation tool to verify the toolpaths and avoid collisions or errors before machining. You will be able to see how the machine will move and where and why you might have issues. Fusion 360 virtually cuts your workpiece mimicking the results you should expect.
• G-Code Generation: After verifying the setup, toolpaths, and reviewing the simulation, post (export) the G-code to control the CNC machine during production. The files generated will be loaded onto the CNC.

Actions and Outcomes for This Module

• Setup Fusion 360 for CAM at VHS: See the section above for detailed instructions.
• Set Up a CAM Project: Define the workpiece and select tools for your CAM project in Fusion 360.
• Create Toolpaths: Develop basic toolpaths and understand different machining strategies such as contouring, pocketing, and others.
• Simulate Toolpaths: Run simulations to verify the correctness and safety of the toolpaths.
• Generate G-Code: Post G-code for use with the CNC machine to execute the operations.
• Instructor Review: Share your CAM setup with the instructor for review before moving to the in-person training. You will need to export your Fusion 360 file as .f3d and send this to the instructor.