Pockets

Fusion provides two different types of pocketing operations. The one called simply “2D pockets” is for traditionalists. It allows you to specify a stepdown and stepover, like a boss.

The other, adaptive clearing, takes the stepover parameter away from you. For adaptive clearing operations, Fusion calculates a toolpath that minimizes load on the bit.

Here are two tool paths for the same pocket, using the same bit. One was created via a 2D pocket operation, the other via adaptive clearing:

Adaptive clearing on the left, 2D pocket on the right.

As you can see, adaptive clearing takes shallower and more curved sidecuts. 2D pockets use parallel cuts with a fixed stepover.

The adaptive clearing tool path is significantly longer than the 2D pocket toolpath, so the machining time is longer as well. Why, then, ever use adaptive clearing?

Because, according to Autodesk, you can make much deeper cuts with each pass. Because the load is lower on the bit, you can afford larger stepdowns without worrying about breaking your bit. How large? Who knows, although anecdotally I’ve been told that 80–90% of flute length is possible.

If you believe this, then adaptive clearing offers potentially greatly reduced machine time for deeper pockets. You’ll have to experiment (and break a few bits) to find out exactly how far you can push things.

Adaptive clearing

Create a pocket cut via adaptive clearing by choosing CAM > 2D > 2D Adaptive Clearing.

Tool tab

Tool

Tool: select tool
For starter projects, there’s a decent chance you will be using either a 1/4" or 1/8" flat end mill, and you don’t need to be concerned with other tool parameters such as material.

Coolant: Disabled
Unless you’re using a coolant, in which case, choose that.

Feed & Speed

Note: I suggest some default feed and speed settings here, but you shouldn’t use these without first having a basic understanding of what these settings are for and how they might differ on your machine.

If you’ve already set up a custom tool library, like I suggested, then you can most likely skip past all these settings and go to the Geometry tab.

Spindle Speed: 8,000 rpm

Surface Speed: Default (calculated for you)

Ramp Spindle Speed: Default (should match spindle speed)

Cutting Feed Rate: chip load * # of flutes * spindle speed
For wood and 1/4" bits: chip load = 0.01
For wood and 1/8" bits: chip load = 0.005

So for a 2-flute 1/4" bit: 0.01 * 2 * 8,000 = 160 inches per minute

Lead-in feed rate: Same as cutting feed rate

Lead-out feed rate: Same as cutting feed rate

Ramp feedrate: Same as cutting feed rate

Plunge feedrate: 50% of cutting feed rate

Geometry tab

Pocket Selections: select the bottom face of the pockets you want to clear

Heights tab

All of the defaults are fine.

Passes tab

Passes

Direction: Conventional
This is another complicated topic, but the limited research I’ve done suggests conventional milling will yield a better finish. If you’re curious, you can always experiment to see if there’s a difference.

Multiple depths

Multiple depths: check
This is how you indicate that you want to step down when clearing the pocket. Otherwise, Fusion will generate tool paths in which the bit plunges straight to the lowest depth of the cut. This is fine if the cut is shallow, but otherwise, you need to enable Multiple Depths.

Maximum Roughing Stepdown: ?
As mentioned up top, Autodesk claims that adaptive clearing allows you to make deeper cuts than you otherwise would with standard pocketing tool paths. The usual advice is to choose a stepdown equal to your bit diameter, but you can experiment with much deeper cuts — up to 80 or 90% of flute length. If you break a bit, you’ll know you went too far.

Stock to leave: unchecked
Unless you plan to do a finishing pass, you don’t want to leave any material when your cut is complete. Uncheck this box to indicate that this cut is meant to be final.

Smoothing: checked
Autodesk claims that smoothing results in better cuts and smaller gcode files, so I generally check this box. Doubt it makes much difference most of the time.

Linking tab

Generally you can take all the defaults here. But if you are cutting pockets that are not much bigger than the width of the bit, you may find that the default ramp type causes problems. Ramping describes how the bit enters the material to reach the cutting depth. The default “Helix” ramp type indicates that the bit will follow a spiral path to enter the material. In the case of very small pockets, the spiral would extend beyond the boundaries of the cut, so Fusion is unable to generate a valid toolpath. To fix, you can try adjusting the size of the helix, or choosing a different ramp type. If need be, the “Plunge” ramp operation represents a straight vertical drop.

2D pockets

As mentioned, the main difference — OK, pretty much only real difference — between 2D pockets and adaptive clearing is that 2D pockets allow you to specify a fixed stepover, rather than use on Fusion’s (supposedly) optimized tool path.

When setting up a 2D pocket, the settings are almost all identical to an adaptive clearing operation. On the Passes tab, make the Maximum Stepover value look OK. It should be set to 40% of bit diameter.

In fact, if it’s not, take this opportunity to update the default. Right-click on the Maximum Stepover field and choose “Edit Expression.” Enter a value of:

tool_diameter * 0.4

Click OK, then right-click on the Maximum Stepover field again, and select “Make Default.”

As mentioned, for 2D pocket operations, the traditional stepdown value is no more than the bit diameter. Here too you can set a default. After you check “Multiple Depths,” go through the same steps as for Maximum Stepover to set the Maximum Roughing Stepdown to:

tool_diameter