Generate Tool Paths

• Tool paths should be generated immediately prior to cutting to ensure bit numbers have not changed.
  • If a tool path takes a long time to generate and/or must be generated in advance, make sure to verify each tool number in the operation vs the tools installed in the machine before starting a cut.
• Utilize template & bit library via Fusion 360 teams (requires invite to proto team) as much as possible
  • Toolpath Template Library
• Check template library for preset operations, for example 2D contour cut in plywood.
  • Make sure to select “Cloud” templates for most up to date feeds & speeds
  • These templates represent previous successful operations and should be utilized whenever possible.
  • Some operations have several bit size options, in general select the largest bit that meets detail requirements of the design.
  • Settings can be adjusted to meet project specific needs, if they differ significantly from the template settings, consider creating a new template.
  • Make sure to clear any “Selected geometries” in templates (if applicable) and update with geometries from current document
  • Templates use the following naming convention
    • Machine Name, Material, Operation Type, Bit Size
• Note, tool numbers in templates are NOT automatically updated and need to be verified against latest installed tools

Toolpaths from Template

• Setup > Create From Template > Select Template
• Make sure “Cloud” templates are selected unless explicitly using a local template
  • Cloud libraries must be enabled “(How to install a cloud tool library)”

• When selecting a contour cut, pay attention to which side of the cut line the bit is on (indicated w/ a red arrow). Clicking on the red arrow will change where the bit cuts relative to the indicated contour line.

  Toolpaths from Scratch

• 2D Adaptive preferred over 2D Pocket, high speed machining (HSM) limits how much of the bit is cutting at a given time, improving tool life and reducing breakage
  • 2D Adaptive Clearing Reference
  • Optimal load: 0.25 x tool_diameter
  • Depth of cut: Max 50% diameter of tool

2D Adaptive

• Critical parameters
  • Tool Tab
    • Feed per tooth
      • Indicates how much material is each revolution by each cutting edge when the machine is performing a normal cut, typical values range from (0.002 to 0.01”)
    • Plunge Feed per Revolution
      • Same as feed per tooth but specific to vertical cutting/drilling, end mills have different geometry than drill bits and are not as efficient cutting straight down into material. Typical values are ~50% of the feed per tooth value (0.001 to 0.005”)
  • 
  • Passes Tab
    • Optimal Load
      • Indicates the maximum amount of tool engagement, as a rule of thumb this value should be approximately 25% of the tool diameter
        • For example, a good starting point for a 3/8” endmill is 0.09375” (0.375 * 0.25)
      • This value can be increased or decrease when machining harder/softer materials (lower for hard materials, higher for soft materials)
    • Maximum Roughing Stepdown
  •