Guide

How to use MillCaliber

Turn a starting estimate into a cut you trust. This guide covers entering your setup, checking the numbers against your tool and machine, running a test cut, and diagnosing what you hear and see.

Last updated 21 October 2026

1. Step by step

  1. Pick the material closest to your stock. If yours isn't listed, don't substitute a “similar” one without checking your tool maker's data.
  2. Pick the cutter diameter and flute count of the tool you will actually use. Use Custom… for other sizes from 0.03 to 1 in (0.8–25.4 mm).
  3. Pick the operation. This pre-fills the width of cut (WOC): 50% for adaptive/pocketing, 100% for slotting, 10% for finishing.
  4. Pick your machine class, then enter your machine's real min and max spindle RPM and max cutting feed. The pre-filled limits are generic.
  5. Set depth of cut (DOC) and adjust WOC if your toolpath uses a different stepover.
  6. Read the notes under the results. They tell you when RPM or feed was limited, when engagement is high, or when the flute count is a poor match for the material.
  7. Open “How this estimate was built” to see each step from the material baseline to the final values.
  8. Copy the CAM values and type them into your CAM tool's speed and feed fields. The copied text is a list of values with units, not a G-code program.

2. Worked example (calculator defaults)

The setup is 6061-T6 aluminum with a 1/4" (6.35 mm) 2-flute carbide end mill, adaptive pocketing, on a desktop belt-driven machine. DOC is 0.25 in (6.35 mm), WOC is 0.125 in (3.175 mm), and the limits are 10,000–24,000 RPM and 200 in/min.

StepImperialMetric
Target surface speed1,200 SFM366 m/min
Ideal RPM = 12 × 1,200 ÷ (π × 0.25)18,335 → 18,00018,335 → 18,000
Intended chip = 0.0023 × 1.000 × 0.55 × 1.000.001265 in0.0321 mm
Chip-thinning factor (WOC = 50%)×1.00×1.00
Cutting feed = 18,000 × 2 × 0.00126545.5 in/min1,157 mm/min
Plunge feed = 30% of cutting feed13.7 in/min347 mm/min
Resulting surface speed1,178 SFM359 m/min
Material removal rate1.423 in³/min23.32 cm³/min

Engagement is (0.5 × 1.0 × 1.00) ÷ 1.0 = 0.50, which is moderate. The feed is well below the 200 in/min limit, so no adjustment is needed.

Now drop WOC to 0.02 in (8% of D). The chip-thinning factor becomes 1.84 and the feed rises to about 83.9 in/min. The tooth still cuts a chip of about 0.0013 in, because the shallow engagement thins it.

Try it in the calculator

3. Check tool and machine limits

  • Tool maker's data first. If the cutter's maker publishes speeds and feeds, use them. If MillCaliber's numbers are higher, use the maker's.
  • Flute length and stick-out. DOC must be shorter than the flute length. Keep stick-out as short as the part allows; deflection grows quickly with stick-out.
  • Spindle range. Trim routers often have speed dials, not RPM readouts. Check your dial-to-RPM table, and enter your true min and max.
  • Feed and acceleration. Enter your controller's max cutting feed. On short moves, slow acceleration means the machine may never reach the programmed feed. That makes the actual chip thinner.
  • Plunging. Not all router bits are center-cutting. Ramp or helix in where possible.
  • Power. MillCaliber doesn't check spindle power. On low-power spindles, if the tone drops or the spindle bogs, reduce DOC first.

4. Test-cut checklist

  1. Use scrap of the same material and thickness, held the way the real part will be.
  2. Wear eye and hearing protection. Have dust extraction or air blast running, and keep a hand near feed hold or e-stop.
  3. Start gentler by reducing engagement, not by slowing the feed alone. Use about half the DOC with the calculated RPM and feed, so each tooth still takes the intended chip. If you change WOC, recalculate in MillCaliber first, because stepover changes the chip-thinning compensation.
  4. Feed override changes chip thickness. Turning the feed override down to 50–75% while the spindle stays at the same RPM makes every chip thinner by the same proportion (for example, 50% feed gives half the chip). That can cause rubbing, heat and fast wear, especially in aluminum, acrylic and hardwood. If you want to slow the whole cut down, lower the spindle speed and the feed by the same percentage so the chip stays the same. Use feed override alone only as a brief safety hold, not as a gentle way to start.
  5. Listen and watch. A steady, even sound, and chips rather than dust or melt, are good signs.
  6. If the cut stays quiet, raise DOC toward your target in steps. If you slowed spindle speed and feed together, bring them back up together.
  7. Stop and check the tool, chips and edge finish. Look for heat, discoloration, built-up material on the cutter, and the wall finish.
  8. Write down the settings that worked. Machine condition changes, so recheck after changing tools, belts or workholding.

5. Diagnosing problems

SymptomLikely causeTry first
Chatter: a loud, rough, rhythmic noise; wavy wallsToo much engagement for the machine's stiffness, long stick-out, loose workholding or a worn toolReduce DOC or WOC. Shorten stick-out and tighten workholding. Try a small RPM change (±5–10%) to move away from a resonance.
Rubbing: squealing, glazed or shiny walls, fine dust, a quickly dulled toolChip too thin: feed too low for the RPM, very small stepover, or feed capped by the machineRaise feed or lower RPM to thicken the chip. Increase WOC. Check for a “chip is thinner than intended” note.
Burning (wood): dark edges, smoke, burn marksTool dwelling, or chip too thin at high RPM; dull bit; poor chip clearingRaise feed or lower RPM. Avoid pauses in the toolpath. Clear chips with an upcut bit or air. Replace dull bits.
Melting (acrylic, plastics): gummy chips, re-welded slot, rough frosted edgeToo much heat: chips too thin, too many flutes, or recut chipsUse a 1–2 flute O-flute cutter. Raise feed or lower RPM so chips are thicker. Clear chips with air. Never dwell.
Chip recutting (especially aluminum): chips packing the slot, built-up edge, poor finishChips not leaving the cut; too many flutes; deep slotUse air blast or mist. Use fewer flutes. Use adaptive clearing instead of full slots. Reduce DOC in slots.
Broken toolOverload, chip packing, plunging with a non-center-cutting tool, or deflectionReduce engagement. Check the notes for high engagement. Ramp instead of plunging. Improve chip evacuation.

6. Feeds vs. speeds explained

Speed is how fast the cutting edge moves past the material. It is set by spindle RPM and cutter diameter, and expressed as surface speed (SFM or m/min). Each material and tool has a range of surface speeds that controls heat and tool wear. MillCaliber starts from a target surface speed and works out the RPM: RPM = 12 × SFM ÷ (π × D).

Feed is how fast the tool moves through the material (in/min or mm/min). It sets the chip load, the thickness of material each flute removes: Feed = RPM × flutes × chip load.

The two must match.

  • A high RPM with a low feed makes thin chips that rub and heat the edge.
  • A low RPM with a high feed makes thick chips that overload the tool.
  • Chips carry heat away, so a correctly sized chip is often cooler than a too-small one.

When you change RPM, change feed by the same ratio to keep the same chip load. When you change stepover, chip thinning changes the real chip; the calculator compensates for this, as described in the methodology.