Dialling In: Chatter, Rigidity and Troubleshooting
Listening to the cut, chatter and stability, rigidity, how to adjust speed and feed one step at a time, and a troubleshooting table.
Listen and look: what the cut is telling you
| What you see or hear | What it usually means | First thing to try |
|---|---|---|
| A steady, even hiss or a smooth hum | A good chip load and speed | Leave it; then raise the feed 10 % |
| A high squeal or scream | Rubbing (feed too low) or a speed on a chatter frequency | Raise the feed; or change the RPM by 10 % |
| A rhythmic thumping or a low growl | Overload, a dull tool or a deep cut | Reduce the depth or the feed |
| A sudden loud chatter with wavy marks | Regenerative chatter | Change the RPM, reduce the stick-out, reduce the depth |
| Chips blue, purple or glowing (steel) | Heat: the speed is too high or no coolant | Lower the speed; add coolant |
| Silver or straw-colored steel chips, curled | Good: heat is leaving with the chip | Keep |
| Dust and fine powder rather than chips | Feed too low, the tool rubs | Raise the chip load |
| Smoke, a burnt smell (wood or plastic) | Feed too low or dull tool | Raise the feed; sharpen |
| Chips welded to the tool (aluminum) | Speed too low or no lubricant | Raise the speed; add lubricant or air |
Rigidity: the chain of springs
Every part between the cutter and the floor flexes: the tool, its holder, the spindle, the machine, the fixture and the workpiece. Their stiffnesses add like springs in series, so the weakest part dominates, and improving a strong part does almost nothing. 1 ÷ ktotal = Σ 1 ÷ ki.
Worked example: a 10 mm end mill in a vise on a knee mill
| Link | Stiffness (N/µm, typical) |
|---|---|
| Tool (10 mm, 30 mm stick-out) | 25 |
| Holder and spindle | 150 |
| Machine structure | 60 |
| Fixture and vise | 100 |
- Total stiffness: 13.6 N/µm: below the tool’s own value. A side force of 120 N deflects the tip by 120 ÷ 13.6 = 8.8 µm.
- Cut the stick-out from 30 to 20 mm: the tool stiffness rises by (30 ÷ 20)³ = 3.4 times to 84 N/µm; the total becomes 22.1 N/µm and the deflection 5.4 µm: shortening the tool beats any upgrade of the strong links.
- Hold the work as close to the cut as you can, use the shortest tool and the largest diameter that fits, and keep the tool holder clean and tight.
Chatter: why it happens
Regenerative chatter is a self-excited vibration. A tooth cuts a wavy surface left by the previous tooth; the chip thickness then varies with the vibration, the force varies with the chip, and the force feeds the vibration. Above a critical depth of cut the vibration grows until the tool jumps, the surface is ruined and the tool may break. The critical depth depends on the structure’s stiffness and damping, and (this is the useful part) on the spindle speed.
- Forced vibration (an unbalanced tool, a worn bearing, runout) shows up at the spindle or tooth-pass frequency and does not grow; chatter is at the structure’s natural frequency and grows with depth.
- A chatter mark pattern that is not related to the feed lines points to chatter; evenly spaced marks per tooth point to runout.
- Remedies, in order: shorter and larger tool; less radial and axial depth; a different spindle speed (the sweet spots below); a variable-helix or variable-pitch tool; stiffer clamping; sharper tool with a lower cutting force.
Finding a stable spindle speed
The stability lobes repeat as the speed changes: the most stable speeds are where the tooth passing frequency is an integer fraction of the structure’s natural frequency fn, because the waves left by successive teeth then line up and cancel. A rough estimate is n = 60 fn ÷ (z k) for k = 1, 2, 3 … (the highest speeds, with small k, give the largest stable depths).
Worked example: speeds to try for a natural frequency of 1 200 Hz
The tool rings at about 1 200 Hz when tapped (the “tap test”: strike the tool and listen to or record the pitch). With 3 teeth the candidate speeds are:
| k | Spindle speed | Tooth-pass frequency |
|---|---|---|
| 3 | 8 000 rpm | 400 Hz tooth-pass |
| 4 | 6 000 rpm | 300 Hz tooth-pass |
| 5 | 4 800 rpm | 240 Hz tooth-pass |
| 6 | 4 000 rpm | 200 Hz tooth-pass |
| 8 | 3 000 rpm | 150 Hz tooth-pass |
- If the cut chatters at 5 400 rpm, try 6 000 rpm (k = 4): the tooth-pass frequency of 300 Hz is 1 ÷ 4 of the natural frequency and the lobe is at a peak. A change of 10 % in the RPM often cures chatter completely.
- You can find the pitch in practice: hum or record the chatter and match it to a note; the loudest sound is at about the natural frequency; then step the RPM towards a sweet spot.
- Low-speed machines gain from the other effect: at very low speed the cutting damping of the tool helps (the process damping), so reducing the RPM by half can also stop chatter.
Dialling in a new job, one step at a time
Starting values (from Speeds and Feeds by Material) are for an average setup. Your machine and tool are not average, so find the real limit by changing one thing at a time and judging the cut each time.
- 1. Begin at the full speed but 70 % of the chip load and a moderate depth. Never start at the top of the range.
- 2. Raise the feed in 10 to 15 % steps (use the feed override on the control) while you listen, look at the chips and feel the part. Stop one step below any sign of overload, squeal or heat.
- 3. Then raise the depth or the stepover in steps and check the power and deflection.
- 4. Adjust the speed last, in 5 to 10 % steps, looking for a quieter, cooler cut and longer life.
- 5. Measure a test part and the tool wear after a few minutes of cutting, and record the final values.
Worked example: raising the feed on a 10 mm four-flute tool
Target chip load 0.08 mm; start at 70 %, and step up by 15 % at 3 183 rpm (100 m/min):
| Step | Chip load | Feed rate | Share of target |
|---|---|---|---|
| Step 1 | 0.056 mm | 713 mm/min | 70 % |
| Step 2 | 0.064 mm | 820 mm/min | 81 % |
| Step 3 | 0.074 mm | 943 mm/min | 93 % |
| Step 4 | 0.085 mm | 1 084 mm/min | 106 % |
| Step 5 | 0.098 mm | 1 247 mm/min | 122 % |
- Five steps take about 15 minutes and find the best feed for the setup; the feed override on the control makes each step a turn of a dial rather than a new program.
- Back off one step from the first sign of trouble and note it: that value is the real limit of the machine, the tool and the material.
The same procedure works for a router or a lathe (see CNC Routers and Hobby Machines and Turning, Threading and Surface Finish).
Setup checklist
- Tool runout under 0.01 mm at the tool: a runout of 0.02 mm makes one tooth cut 0.08 mm and the next 0.04 mm instead of 0.06 mm: 33 % more load on one tooth, and a short life.
- Tool length: stick-out as short as the cut allows (under 3 × D if possible).
- Holder, collet and spindle taper clean; torque the collet nut properly.
- Work held rigidly and as close to the cut as possible (see Workholding and Fixturing).
- Coolant or air aimed at the edge, chips clear.
- Speed and feed overrides at 100 % to start; the program has the right feed units and tool number.
- Dry run the program above the work, then a first part at 70 % of the feed with a hand near the stop (see Machine and Hand Tool Safety).
- Write down the final values in a job log or a library of tested values.
Troubleshooting table
| Symptom | Likely causes | Try, in this order |
|---|---|---|
| Chatter (wavy marks, loud noise) | Too much depth, long stick-out, unstable speed, loose work | Shorter tool, less depth, a different RPM, better clamping, variable-helix tool |
| Tool breaks | Chip load too high, depth too deep, packed chips, runout, hard spot | Lower the feed and depth, clear chips, check runout and stick-out |
| Tool wears fast | Speed too high, no coolant, rubbing (feed too low), wrong grade | Lower the speed 20 %, raise the feed, add coolant (see Tool Life, Wear and Cutting Economics) |
| Built-up edge, chips welded on | Speed too low, gummy material, dull edge | Raise the speed, sharp polished tool, lubricant |
| Poor surface finish | Feed too high for the nose or corner radius, chatter, wear, runout | Finishing pass with a small stepover, check wear and rigidity |
| Part is the wrong size or tapered | Tool deflection, thermal growth, wear | Spring pass, shorter tool, coolant, offset for wear |
| Burn marks (wood, plastic) | Feed too low, dull tool, slow RPM for the feed | Raise the feed or lower the RPM; sharpen |
| Spindle slows or stalls | Overload | Reduce the depth first (see Cutting Force, Power and Torque) |
| Burrs on the exit edge | Dull tool, no back-up, feed too high at the exit | Climb milling, sharper tool, lighter last pass, deburr |
| Corners overload or chip | Engagement jumps in an inside corner | Slow the feed in corners, use an adaptive path (see Chip Load, Chip Thinning and Engagement) |
Related
- Speeds and Feeds: the overview of this guide.
- Cutting Speed, Spindle Speed and Feed Rate: the formulas to recalculate with.
- Cutting Force, Power and Torque: power, torque and deflection.
- Troubleshooting, Accuracy and Safety (CNC Machining) and the CNC Feeds and Speeds Calculator.
FAQ
How do I stop chatter?
Shorten the tool and hold the work closer, reduce the depth, change the spindle speed by about 10 % towards a sweet spot, and use a variable-helix tool; the cut and the rigidity chain tell you which.
Should I change speed or feed first?
Feed first: raise it in 10 to 15 % steps from 70 % of the target; change the speed last, in small steps, one thing at a time.
Why does a small change in RPM fix chatter?
Chatter depends on how the waves from successive teeth line up; at the right speed the tooth-pass frequency is a fraction of the natural frequency and they cancel, so a 10 % change moves you from a trough to a peak of the stability lobes.
How much runout is acceptable?
Under about 0.01 mm at the tool; a runout of 0.02 mm on a 0.06 mm chip load makes one tooth cut 33 % more than the other.
References
- Altintas, Y., Manufacturing Automation: Metal Cutting Mechanics, Machine Tool Vibrations and CNC Design, Cambridge University Press (chatter and stability lobes).
- Smith, S. and Tlusty, J., Efficient Simulation Programs for Chatter in Milling, CIRP Annals (1993); Tlusty, J., Manufacturing Processes and Equipment, Prentice Hall.
- Machinery’s Handbook and the tool maker’s troubleshooting guides (Sandvik, Kennametal, Harvey Tool).
Last reviewed: October 2026. The stiffnesses, frequencies and the sweet-spot estimate are illustrative: measure your own tool and machine.