Feeds and Speeds

Overview#

Feeds and speeds determine whether a cut is smooth, fast and tool-friendly, or noisy, slow and destructive. The terms:

• Surface speed (Vc): how fast the cutting edge moves relative to the material, in meters per minute (m/min) or surface feet per minute (SFM). It is a property of the tool material and workpiece material pairing, not of the machine.
• Spindle speed (n): rotations per minute (rpm). Derived from surface speed and tool diameter.
• Feed per tooth (fz): the chip load; how far the tool advances per flute per revolution.
• Cutting feedrate (vf): table travel speed during a cut, in mm/min or in/min. Derived from spindle speed, flutes and fz.
• Feed per revolution (fn): how far the tool advances per spindle revolution (turning and drilling use it heavily).

The relationships (metric):

n  = (Vc * 1000) / (pi * D)
vf = n * z * fz
fn = z * fz

where D is diameter in mm, z is flute count. In inch units, n = (SFM * 12) / (pi * D).

Fusion exposes these on the tool's Cutting data tab and on each operation's Tool tab. Autodesk notes you can enter cutting data, or use Surface speed and Use feed per revolution to calculate the speeds and feeds.

Warning: Fusion calculates arithmetic; it does not know your machine. Spindle power, rigidity, tool stick-out, workholding and coolant all limit what is achievable. Treat any calculated number as a starting point.

Where to find it#

• Tool editor > Cutting data tab: saved with the tool as one or more presets.
• Operation dialog > Tool tab: lists the tool, the active Preset, and the cutting-data fields, which can be overridden for that operation only.
• Manage > Tool Library: edit presets (right-click the tool > Edit tool) without opening an operation.

The cutting-data parameters#

The tool's cutting data is grouped as Speed (spindle speed, surface speed, ramp spindle speed), Feedrates (cutting, feed per tooth, lead-in, lead-out, ramp), Vertical feedrates (plunge, feed per revolution) and Passes and linking (stepdown, stepover, coolant). Some operations have their own extra feed fields (for example a transition feedrate on certain strategies) in their Passes or Linking tabs.

Note: not confirmed in Autodesk's documentation: whether feed-per-revolution output produces G95 in the posted code; that depends on the post.

Choosing starting values#

Surface speed by material (guidance only)#

These are widely published starting ranges for carbide tooling and moderate-engagement cuts. They are not from Autodesk and not guaranteed. Always consult your tool manufacturer's data.

If your spindle cannot reach the rpm that a given surface speed implies (common on small machines with a 10,000 rpm limit), you scale the rpm down and, to preserve chip load, scale the feed down proportionally.

Chip load (fz) by tool diameter#

Chip load grows with tool diameter. As a rough aluminum guide: about 0.02 to 0.04 mm for 3 mm tools, 0.04 to 0.08 mm for 6 mm, and 0.06 to 0.12 mm for 10 to 12 mm. For steel, reduce by 30 to 60 percent. Again, defer to your tool vendor's chart.

If chip load is too low, the tool rubs instead of cutting. Heat builds and the edge wears quickly, especially in work-hardening alloys. If too high, the tool deflects, chatters, or breaks.

Chip thinning and stepover#

With a low radial engagement (stepover) the actual chip is thinner than the programmed fz because the flute enters and exits the material with a shallow angle. To keep a real chip load, feed should be increased as radial engagement falls.

For a straight end mill with radial engagement ae less than half the diameter, the chip thinning compensation factor is approximately:

factor = D / (2 * sqrt(ae * (D - ae)))

(valid for ae below D/2; at ae = D/2 the factor is 1.) For example, with a 10 mm tool and ae = 1 mm: 10 / (2 * sqrt(1 * 9)) = 1.67. The feed can be raised by about 67 percent for the same actual chip thickness.

Adaptive roughing, which uses small radial engagements and deep axial engagement, relies on this idea. Fusion's separate Feed Optimization option (Passes tab) does something different: it reduces the feedrate in sharp corners, using Maximum Directional Change, Reduced Feed Radius, Reduced Feed Distance, Reduced Feedrate and an Only Inner Corners checkbox. It does not apply chip thinning compensation.

Tip: When you program a shallow-stepover finishing pass, do not leave fz equal to your roughing value and call it done. The chip is thinner, and a feed boost improves tool life and surface finish.

Presets#

A preset is a named bundle of cutting data stored with a tool. A good workflow:

1. Create the tool.
2. Add presets per material and per operation class: "Alu rough", "Alu finish", "Steel rough", "Steel finish".
3. Fill spindle speed or surface speed, feed per tooth, and the plunge, lead-in/out and ramp feeds.
4. In operations, pick the matching preset. The operation's Preset dropdown loads the values.

Typical relationships for supporting feeds (general industry rules of thumb, not Autodesk data; adjust to your setup):

Step by step: set up cutting data#

1. Open the tool in Manage > Tool Library (right-click > Edit tool).
2. Switch to the Cutting data tab and click Add preset.
3. Name it, for example "Aluminum 6061 rough".
4. Enter Surface speed 250 m/min. Fusion computes spindle speed from tool diameter.
5. Enter Feed per tooth 0.08 mm. Fusion computes cutting feedrate using flute count.
6. Set Plunge feedrate at 30 percent and Ramp feedrate at 60 percent of cutting feed; set Lead-in/out to the cutting feed.
7. Choose a Coolant type your machine supports.
8. Click Accept.
9. In the operation, choose the preset. Check that the spindle speed fits your machine range. If the machine caps at 12,000 rpm, set the spindle to 12,000 and reduce the feed to keep chip load: edit fz, not only rpm.

Worked example#

A 10 mm, 3-flute carbide tool in aluminum. Vc = 300 m/min.

n  = 300 * 1000 / (pi * 10) = 9,549 rpm
fz = 0.08 mm
vf = 9,549 * 3 * 0.08 = 2,292 mm/min

Your machine maxes at 8,000 rpm. Keep fz at 0.08:

vf = 8,000 * 3 * 0.08 = 1,920 mm/min

The actual surface speed is 251 m/min, which remains fine for aluminum.

Drilling example#

A 6 mm drill in mild steel, Vc = 30 m/min, fn = 0.10 mm/rev:

n  = 30 * 1000 / (pi * 6) = 1,592 rpm
vf = 1,592 * 0.10 = 159 mm/min

Machine and process limits#

Calculated numbers hit real limits:

• Spindle max rpm and torque curve: low rpm on large tools lacks torque; high rpm on small tools lacks power (varies by spindle type).
• Feed limit: table acceleration and the controller's look-ahead cap real feed in tight toolpaths. If your toolpath has many short segments, the machine slows regardless of programmed feed.
• Rigidity: stick-out cubed influences deflection. A tool sticking out three times its diameter is much more flexible than one sticking out twice its diameter. Reduce depth or feed with long stick-out.
• Coolant and chip evacuation: deep pockets with poor chip clearing can recut chips and break tools. Use air blast or flood/through-tool coolant.
• Machine class: desktop machines (spindle power in the hundreds of watts to a couple of kilowatts) will limit stepdown and stepover much more than a VMC.

Note: not confirmed in Autodesk's documentation: whether attaching a machine to a setup clamps cutting values to the machine's spindle limits. Check the posted spindle speeds yourself.

Options reference#

Tips and pitfalls#

Tip: Change one variable at a time while tuning. Increase feed first (watch sound and chip color), then stepover or stepdown. Keep notes on what worked per material and machine; store the results as presets.

Tip: Look at chips. Small powdery chips mean too little chip load. Long, stringy, hot, blued chips in steel mean too much heat. Well-formed chips that leave warm but not hot are a good sign.

Tip: Review ramp, lead-in and plunge feeds in each operation; values left at low defaults slow the cycle. Feed Optimization segments are highlighted in dark yellow on the toolpath.

Warning: Linked fields can surprise you. If you type a new spindle speed while surface speed is linked to it, cutting feed may change. After editing, review all values.

Warning: A feedrate too high for the controller's rapid or maximum axis speed is clamped or alarms depending on the control. Check the machine's maximum feed.

Warning: Inch versus metric. A feed of 1920 interpreted as in/min would be a catastrophic mistake. Confirm units in the posted code and on the control.

Note: not confirmed in Autodesk's documentation checked for this page: any feed or rapid limits under Personal-use licensing; see the manufacturing extensions page.

Practice exercise#

Create a 6 mm 2-flute carbide flat end mill. Add two presets:

• "Alu slot" with Vc 200 m/min, fz 0.04 mm.
• "Steel contour" with Vc 70 m/min, fz 0.02 mm.

Compute rpm and feed by hand using the formulas and compare to Fusion's values (rounding differences are normal). Then apply a 12,000 rpm limit to "Alu slot" and recompute the feed to keep fz at 0.04.

Expected values: Alu slot n = 10,610 rpm, vf = 849 mm/min (below the limit); Steel contour n = 3,714 rpm, vf = 149 mm/min.

Related#

• Tools and tool libraries: where presets live
• Pocket and adaptive roughing: low-engagement feeds in practice
• Face and contour: finishing passes and feed
• Toolpath simulation: reviewing feeds and cycle time