Mill Toolpath Guide

CNC Milling is essentially taking a big block of metal and turning it into (nearly) whatever you want. It is a subtractive manufacturing method, compared to additive manufacturing (aka 3D printing). This means that material can only be removed, not added. CAM software is used to program CNC machines to make your part. Fusion 360 is the standard CAM software at BIDC. You create CAM by making a series of toolpaths that form your part. This page focuses on the toolpaths themselves. If you are just starting your CAM, you will need to do some setup with your CAD model and the BIDC workholding. Watch this playlist of videos to get started on your setup, then refer to this page to create the toolpaths for your part! To learn more about what each tool is called, refer to the Mill Tooling Guide. To learn more about the workholding, and how your part will be clamped in the CNC mill while being machined, refer to the Workholding Guide.

Definitions

  • CNC: Computer Numerical Control, refers to machines that are pre-programmed and controlled by computers, rather than manual control
  • CAM: Computer-Aided Manufacturing, the software that allows you to program toolpaths that control CNC machines. BIDC uses Fusion 360 for creating CAM.
  • Toolpath: A pre-calculated path a tool will take to cut out a particular geometry.
  • Speed: How fast the tool spins in RPM (think S for Spin).
Image showing an endmill spin direction
  • Feed: How fast the tool moves linearly across the table in in/min (think F for Forward).
Image showing an endmill feed direction
  • Stepover: How much a tool cuts sideways in a single cutting pass.
Image showing an endmill stepover
  • Stepdown: How deep the tool cuts in a single cutting pass.
Image showing an endmill stepdown
  • Stock: The raw block of material you will make your part out of.
  • 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)

Minor Notes

You can set many of the settings for each toolpath to be dependent on Expressions, which will adapt based on the selected tool’s parameters. You can click on the 3 vertical dots next to a parameter and click [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

Each tool has its speeds and feeds precalculated for you. We use the Kennametal Novo Tool to determine these speeds and feeds. Feel free to explore this and ask a TA for more information.

Probing

The CNC Mill first needs to figure out where your stock is located on the machine. We typically cannot place stock in the machine exactly where it is within CAM (to within 0.001″) by hand. So, probing will almost always be the first toolpath in your setup. The probe will physically make contact with your part to find certain surfaces. If the probe touches two parallel surfaces, it will find the center point between them. We can also probe later in the operation to get better accuracy or determine deviations from expected part geometry. The probe tool itself is loaded in every CNC Mill in tool slot #20.

When it comes to what to probe, usually you probe off your stock on the first operation, and off the machined surfaces of your part/the vice for subsequent operations. As said before, stock usually isn’t very square. If you probe off the stock on the second operation, there is a chance your features from op2 won’t be aligned with those from op1. So, you want to probe off trusted surfaces. If your part’s machined surfaces are resting flat in a vice, then you can trust that probing off of the vice (most commonly in the z-axis) will ensure your toolpaths will align with where your part actually is. Just think about what is being probed, and how that locates where the machine will run the toolpaths.

GIF of the CAM view of the probing toolpath

To create your probe toolpath, use the probing template! Right-click on your setup, select “Create from Template”, then “Select Template”, and click on “XYZ Probing.” This will automatically generate two named toolpaths (one for Z-probing and one for XY-probing) with the correct settings, so all you need to do is select the geometry you want to probe. If the template is missing from the cloud and the probing toolpath must be made manually, the following settings are what you need to set.

Image showing how to get to the probing template in Fusion 360
  • Probe WCS Settings
    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)
      Image showing the geometry tab and selections to make for the probing toolpath
    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 (-0.125in works well)
      Image showing the bottom height selection for a XY probe toolpath
    4. Actions: Check [Override Driving WCS] and change the WCS Offset to 2
      Image showing the WCS settings for a probe toolpath
    5. Repeat for additional axes

2D Operations

The 2D set of toolpaths in Fusion 360 are the most basic but often used toolpaths. In most case, most if not all of your toolpaths will be from the 2D section.

Facing: This toolpath essentially just flattens the stock. You may measure your part’s height with calipers, but there still may be some uncertainty in this dimension. Additionally, your stock might be warped and the height is not consistent along its length. Facing removes this uncertainty by taking off the whole top of the material.

GIF of the CAM view of the facing toolpath
  • Facing Settings
    1. Tool: suitable shell mill for material, Stellram or Dodeka
      Image showing the tool selections for a facing pass
    2. Geometry: [Stock Contours], [Stock Selections] = [Nothing] for basic facing, select geometry if you only want to face a certain area.
      Image showing the geometry selections for a facing pass
    3. Passes: Stepover – [2/3 of the tool diameter], (Edit Expression to tool_stepover)
      Image showing the stepover selections for a facing pass
    4. Check [Multiple Depths] set to [0.050”], (Edit Expression to tool_stepdown)
      Image showing the stepdown selections for a facing pass

2D Adaptive Clearing: A roughing pass that removes most of the stock material to get the general shape of the part. The exact path the tool takes is calculated by Fusion to ensure that the tool load is consistent throughout the whole operation. This is a very common operation. It is typically done with an endmill. Since it is just roughing, we use the largest endmill that works, as that will be the fastest. We can have subsequent 2D adaptive passes with a smaller endmill to get into corners/places the larger endmill could not. However, if your workholding isn’t very rigid, then using a large tool may send the part flying out of the vice. So if you are worried about a lack of clamping force, use a smaller tool to reduce those cutting forces.

GIF of the CAM view of a 2D Adaptive Toolpath
  • 2D Adaptive Clearing Settings
    1. Tool: Largest endmill to fit geometry, shorter is better
      Image showing the tooling selections for a 2D adaptive cut
    2. Geometry: Select the bottoms of the pockets/features to remove
      Image showing the geometry selections for a 2D adaptive cut
      • Click the red arrow if it is cutting the wrong side
    3. Passes: Optimal Load = [10% of tool diameter], (Edit Expression to tool_stepover)
      Image showing the selections for optimal load on a 2D adaptive cut
    4. Check [Multiple Depths] – [90% of flute length], (Edit Expression to tool_stepdown)
      Image showing the selections for multiple depths on a 2D adaptive cut
    5. Check [Stock to Leave] – Axial stock to leave = [0”], Radial stock to leave = [0.020″]
      Image showing the selections for stock to leave for a 2D adaptive cut

2D Contour: A toolpath that follows the selected contour. It is typically used as a finishing pass for a good surface finish. If used like this, set the feed rate to “slotting,” which slows down the tool’s feedrate. For the finishing pass to work, in the preceding 2D adaptive, have “Stock to Leave” selected, allowing the 2D adaptive to leave a little extra material for the finishing pass to cut. This toolpath is typically done with an endmill.

GIF of the CAM view of a 2D contour
  • 2D Contour Settings
    1. Tool: Largest endmill to fit geometry, shorter is better
      Image showing the tooling for a 2D contour
    2. Change cutting preset to slotting
      Image showing the slotting speed selection for 2D contours
    3. Geometry: Select the contour to cut along, contours can be open or closed loops
      Image showing the geometry selection for a 2D contour
    4. Passes – Compensation Type = [In Control]
      Image showing the in control selection for a 2D contour`
      • Note: tool diameter must be probed

Slot: A toolpath follows the centerline of a closed slot and cuts downwards in a ramping fashion. This toolpath will use the full width of the endmill, so it requires “slotting” speeds and feeds and cannot machine very deep per stepdown. For an open slot (the tool starts outside the part and gets through to the other side), use a 2D contour with slotting settings.

GIF showing the CAM view of the slotting toolpath
  • Slot Settings
    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 stepdown of [10% tool diameter].

Bore: Makes a hole that is larger/in a different size than available drills. It is a spiral entry of an endmill and is typically used with that tool. You might notice that the 2D adaptive toolpath automatically uses boring to enter into the material as well.

GIF of the CAM view of the boring toolpath
  • Bore Settings
    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: A toolpath that engraves a sketch onto a part. The depth of the engraving is based on the distance between two sketch lines, so it adapts its height as it cuts.

GIF of the CAM view of the engraving toolpath
  • Engrave Settings
    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: A toolpath that follows a contour and creates a given size chamfer. Note that this only works if the chamfer is not modeled. If a chamfer was modeled, suppress the chamfer in the CAD. You can adjust the size of the chamfer to whatever size you desire but do not model it for manufacturing.

GIF of the CAM view of the chamfer toolpath
  • Chamfer Settings
    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

Drilling

Drilling is used to make holes. While you can bore out hole sizes with an endmill, it is much easier and faster to use a drill to make the hole. So, try to size your holes to fit to those in our drill library! Know your tool material for drills. If using a carbide drill, you need a flat surface. A carbide drill cannot do any form of pecking, so it must go straight down to the bottom of the hole without stopping. Use Through-Spindle Coolant if the machine supports it. You cannot use a carbide drill for creating a counterbore, or if two holes meet each other. If using HSS, you will need to create a dimple/spot hole for the drill to guide it in. You can use a spot drill or a carbide drill for this. You also need to set the drill type to a pecking of some sort. For larger-size HSS drills, drilling out the hole completely with a smaller-size drill is also advisable.

GIF of the CAM view of the drilling toolpath
  • Drill Settings
    1. Tool: Drill of the desired diameter, shortest length possible for hole depth
      Image showing the drill tool libraries
    2. Geometry – Hole Faces, select holes to be drilled, use [Select Same Diameter] for repeated holes
      Image showing the geometry selections for a drilling toolpath
    3. For Thru Holes: Heights – Bottom Height – [Drill Tip Through Bottom], add a small Offset
      Image showing the "drill tip through bottom" selection for the drilling toolpath
      • NOTE: IF THE HOLE IS COUNTERBORED, YOU MUST SELECT THE TOP OF THE PART: Heights: [Top Height] – [Model Top]
    4. Cycle – Cycle Type [Drilling – rapid out] for carbide drills (GoDrills) or [chip breaking – partial retract]/[deep drilling – full retract] for HSS drills.
      Image showing the cycle type selections for a drilling toolpath

3D Operations

3D Adaptive: An adaptive clearing toolpath that adjusts for whatever geometry you have. Use this for when 2D work won’t due to complex 3D geometry.

GIF of the CAM view of a 3D Adaptive toolpath

IMPORTANT CAVEATS: 3D adaptive, while powerful, requires extra oversight when creating the toolpaths to ensure there are no potential crashes. Unlike 2D adaptive, where you select contours and faces that you want to machine, 3D adaptive looks at the part geometry and makes its own decisions. 3D adaptive is more flexible, at the cost of removing control you had over your toolpath. There are two very important selections you need to make: Boundary Selection and Bottom Height.
Boundary Selection: This selection constrains the horizontal locations the tool can cut inside. By default, this boundary is set to nothing, so the 3D adaptive will attempt to machine the entire part. With the default Bottom Height set to Model Bottom, this can very easily lead to crashes with your workholding. Many times, you don’t want the 3D adaptive to machine the entire part. So, you make a boundary selection to only machine the features you want made with this toolpath. You can select tool inside, tool on, or tool outside boundary to adjust where the tool stops at the boundary.
Bottom Height: This selection is also very important. By default, it is set to the bottom of your model. Many times, you don’t need this and only need to go down enough to machine a particular feature. So, set this only as low as you need it to do, and not any lower. If you are doing an exterior adaptive, then make sure your bottom height selection is above the height of your jaws. Probe off your jaws if needed to ensure it doesn’t crash.

In general, use 2D adaptive for everything you realistically can, then use constrained 3D adaptives to get the tougher parts of your part. If your part has smoothed, complex contours, then a 3D adaptive is required. But make sure you wisely set up your toolpath settings so there are no crashes.

  • 3D Adaptive Settings
    1. Tool: largest endmill to fit geometry, shorter is better
      Image showing the tooling selection for a 3D adaptive
    2. Geometry: Select the outside boundary of desired features
      Image showing the machining boundary selections for a 3D adaptive
    3. Heights: Ensure [Bottom Height] selection is not at the default [Model Bottom], but is limited to how deep you actually need for the particular toolpath.
      Image showing the bottom height selections for a 3D adaptive
    4. Passes – Optimal Load = [10% of the tool diameter]
      Image showing the optimal load for a 3D adaptive
    5. Maximum Stepdown – [90% of flute length]
      Image showing the maximum roughing stepdown for a 3D adaptive
    6. Fine Stepdown, like the resolution of the process, at your discretion
      Image showing the fine stepdown settings for a 3D adaptive
    7. Check [Stock to Leave] – leave default values
      Image showing the stock to leave settings for a 3D adaptive

3D Finishing (scallop, step and shallow, etc.): There is a whole range of toolpaths that are designed for finishing 3D contours. These will typically use an endmill and conform to your geometry. Make sure most of the material is roughed away with 3D adaptive before using these toolpaths. The strategies are all largely similar, it is recommended to use [Steep and Shallow] unless a specific path is preferred

Image of the CAM view of a scallop toolpath
  • 3D Finishing Settings
    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 stepdowns you need, usually one or two]

Multi-Axis Operations

There are a couple of multi-axis toolpaths within Fusion 360 for use on the 5-axis. For some of the 3D finishing operations, you will have the ability to turn those into multi-axis toolpaths. There are also some dedicated multi-axis toolpaths. Ask a BIDC Metal Shop TA for more help in setting up 5-axis operations.

Further Toolpaths

Fusion 360 has many more toolpaths than what was covered here! These just represent the most common ones. If you want to learn more about a particular toolpath, all you need to do is hover your mouse over the toolpath, and a window will pop up explaining how it works.

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
  • If the 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, so being more conservative with your toolpaths is best.