mill toolpath guide

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.

Facing Settings

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], (Edit Expression to tool_stepover)
   
4. Check [Multiple Depths] set to [0.050”], (Edit Expression to tool_stepdown)
   

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.

2D Adaptive Clearing Settings

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: 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.

2D Contour Settings

1. Tool: Largest endmill to fit geometry, shorter is better
   
2. Change cutting preset to slotting
   
3. Geometry: Select the contour to cut along, contours can be open or closed loops
   
4. Passes – Compensation Type = [In Control]
   
   • 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.

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.

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.

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.

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

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.

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
   
2. Geometry: Select the outside boundary of desired features
   
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.
   
4. Passes – Optimal Load = [10% of the tool diameter]
   
5. Maximum Stepdown – [90% of flute length]
   
6. Fine Stepdown, like the resolution of the process, at your discretion
   
7. Check [Stock to Leave] – leave default values