• Tooling Note: Tools are organized by machine compatibility
• Cutting Presets: Each tool has all materials it can cut organized into categories
  • N – Nonferrous, P – Steel, M – Stainless Steel, S – Superalloys, H – Hardened Materials
  • See Material ISO grades to identify your material (anything from the stock room is usually aluminum N2 or mild steel P0)
• Edit Expression and change User Defaults for easy use
  • Fusion has a ton of variables that you can use for making toolpaths, you can right click on number boxes and [Edit Expression] to type in parameters like tool_stepover and tool_stepdown for values like Stepover/Optimal Load and Stepdown, respectively. Then save as user default
• Kennametal’s Novo Tool lets you calculate custom speeds and feeds for our tooling, check the library or ask us for more info

Probing

• Probe WCS (USE THE TEMPLATE IT’S MUCH EASIER)
  1. Tool: Work Probe
     • Lead-In Feedrate can be increased to a maximum of 100in/min, 50 is recommended
  2. Geometry: whatever surfaces you would like to reference, you can select the top surface and change it to probe XY or probe Z surface, or select vertical surfaces directly (ask if you’re not sure)
  3. Heights: Change the bottom height to [From Probing Surface Top] and adjust the offset to make sure the ball of the probe tip makes full contact with the probing surface (-0.1in works well)
  4. Actions: Check [Override Driving WCS] and change the WCS Offset to 2
  5. Repeat for additional axes

2D Operations

• Facing
  1. Tool: suitable shell mill for material, Stellram or Dodeka
  2. Geometry: [Stock Contours], [Stock Selections] = [Nothing] for basic facing, select geometry if you only want to face a certain area.
  3. Passes: Stepover – [2/3 of the tool diameter]
  4. Check [Multiple Depths] set to [0.050”] (or [0.100”] in aluminum)
• 2D Adaptive Clearing (Trochoidal Milling)
  1. Tool: Largest endmill to fit geometry, shorter is better
  2. Geometry: Select the bottoms of the pockets/features to remove
     • Click the red arrow if it is cutting the wrong side
  3. Passes: Optimal Load = [10% of tool diameter], (Edit Expression to tool_stepover)
  4. Check [Multiple Depths] – [90% of flute length], (Edit Expression to tool_stepdown)
  5. Check [Stock to Leave] – Axial stock to leave = [0”], Radial stock to leave = [0.020″]
• 2D Contour
  1. Tool: Largest endmill to fit geometry, shorter is better
  2. Geometry: Select the contour to cut along, contours can be open or closed loops
  3. Passes – Compensation Type = [In Control]
     • Note: tool diameter must be probed
• Slot
  1. Tool: Largest endmill to fit geometry, shorter is better
  2. Change cutting preset to SLOTTING!
  3. Geometry: Select the bottom contour of the slot
  4. Passes: Check [Multiple Depths], [Maximum Roughing Stepdown] = [tool diameter], (Edit Expression to tool_stepdown)
• Bore
  1. Tool: Endmill approximately 2/3 the diameter of the desired hole, shorter is better
  2. Change cutting preset to slotting
  3. Geometry: Select Hole Face, check [Select Same Diameter] for multiple holes
• Engrave
  1. Tool: small Chamfer Mill or Ball Mill
  2. Geometry: Select the curve to cut along
  3. Heights – Bottom Height = [Depth of the engraving (negative value)]
  4. Passes – Multiple Depths = [25% of tool diameter]
• Chamfer
  1. Tool: Chamfer Tool (listed as Other Toos)
  2. Geometry: Select the contour to cut along
  3. Passes: Chamfer Width [Depth of chamfer down the side of the part]
  4. Passes: Chamfer Tip Offset = [0.050″]
• Set Proper [Tool Orientation] under [Geometry] tab if applicable for Multi-Axis machining

3D Operations

• 3D Adaptive – only for when 2D adaptive does not work for complex geometry
  1. Tool: largest endmill to fit geometry, shorter is better
  2. Geometry: Select the outside boundary of desired features
  3. Passes – Optimal Load = [10% of the tool diameter]
  4. Maximum Stepdown – [90% of flute length]
  5. Fine Stepdown, like the resolution of the process, at your discretion
  6. Check [Stock to Leave] – leave default values
• 3D Finishing Strategies are all largely similar, it is recommended to use [Steep and Shallow] unless a specific path is preferred
  1. Tool: largest ball mill to fit geometry, shorter is better
  2. Geometry: Select the outside boundary of desired features, can be tricky, try a tutorial!
  3. Passes: [Stepover], like the resolution of the process, at your discretion, finer stepover takes more time
     • 0.030″ rough, 0.015″ medium, 0.005″ fine, 0.001″ extra fine
• Project; Engrave onto a curved surface
  1. Tool: small Chamfer Mill or Ball Mill
  2. Geometry: Select the curve to cut along
  3. Passes: Axial Offset = [Depth of the engraving (negative value)]
  4. Check Axial Offset Passes
  5. Maximum Stepdown = [25% of tool diameter]
  6. Number of Stepdowns = [However many stepdown you need, usually one or two]

Drilling

• Drill
  1. Tool: Drill of the desired diameter, shortest length possible for hole depth
     • Additional Sizes available at Bechtel Center
  2. Geometry – Hole Faces, select holes to be drilled, use [Select Same Diameter] for repeated holes
  3. For Thru Holes: Heights – Bottom Height – [Drill Tip Through Bottom], add a small Offset
     • NOTE: IF THE HOLE IS COUNTERBORED, YOU MUST SELECT THE TOP OF THE PART: Heights: [Top Height] – [Model Top]

Multi-Axis Operations

• Set Proper [Tool Orientation] under [Geometry] tab if applicable
• Swarf
  1. Tool: largest endmill to fit geometry, shorter is better
  2. Geometry: Surfaces to cut
     • Click the red arrow if it is cutting the wrong direction
• NOTE: A-Axis must be reversed in post-processor settings

Troubleshooting

• Review the simulation to check for any crashes
• Warning that a height was raised or a lead in/out was modified: Not a problem
• Rapid Collision with Stock: Check heights and selected geometry
• Toolpath not doing what you want it to: Try another toolpath or mess around in Passes

Note: this is a simulation that can do unrealistic things with tools that will break them, conservative is best.