How to Change Feed and Speeds on a CNC Machine
Most operators change feed and speeds on a cnc machine by copying the last job or the tool catalog. That works until it does not. This guide shows how to set them from first principles: calculate a starting point, prove it on the machine, then correct it with evidence. Written for engineers and setup machinists who need parts in tolerance, not a lecture on cutting theory.
In this article
- 1
- 2
- 3
- 4
- 5
- 6
- 7
- 8
Key takeaways
What surface speed and chip load actually mean
Two numbers drive everything on the control. Surface speed (Vc, in m/min or sfpm) is how fast the cutting edge travels through the material. Chip load (fz, in mm/tooth or in/tooth) is how thick each tooth's slice should be. Spindle rpm comes from surface speed divided by tool diameter. Feed rate comes from chip load multiplied by tooth count and rpm.
This split matters because the two numbers fail differently. Run surface speed too high on 6061 and you get built-up edge and a gummy finish. Run it too high on Ti-6Al-4V and the insert edge breaks down in minutes. Run chip load too low and the edge rubs instead of cuts, which raises temperature and work-hardens stainless. Run it too high and the tool deflects or snaps.
Tool diameter changes rpm fast. A Ø12 mm carbide end mill at 120 m/min runs about 3,180 rpm. The same surface speed on a Ø3 mm tool needs roughly 12,700 rpm. If your spindle tops out at 12,000 rpm, you cannot hit that surface speed, so you compensate with a lower chip load and a slower feed. That is normal, not a mistake.
Materials set the window. Aluminum 6061 tolerates 300–500 m/min with coated carbide. 304 stainless sits near 120–180 m/min. Ti-6Al-4V runs 40–60 m/min. Inconel is lower still, often 25–35 m/min with flood coolant. Use the maker's starting values, then adjust for your setup.
- 1Surface speed sets rpmrpm = (Vc × 1000) / (π × D) for metric.
- 2Chip load sets feedFeed = fz × teeth × rpm.
- 3Diameter scales rpm inverselyHalf the diameter, roughly double the rpm.
Reading a tool catalog without getting burned
Catalog charts assume a rigid setup, a new tool, and a specific coating. Your machine may be a 3-axis mill with 500 × 500 × 450 mm travel, or a 5-axis center with a Ø400 mm rotary table. The smaller machine will flex earlier. Start at roughly 70 percent of the catalog feed and speed, cut one pass, then step up in 10 percent increments.
Radial and axial engagement change the load on the tool. A 50 percent radial stepover at full depth is far heavier than a 10 percent stepover with a long axial cut. Many shops now use high-efficiency milling: light radial engagement, deep axial passes, higher feed per tooth. This lowers radial force and lets a small machine remove material without chatter.
Coolant strategy is part of the number. Aluminum likes flood or high-pressure through-spindle coolant to clear chips. Titanium needs flood to control heat. Cast iron often runs dry. If you switch coolant off, expect to drop surface speed by 20–30 percent and watch the chip color closely.
Tool life is the feedback signal. If an insert dies after 20 minutes instead of 60, surface speed is usually the cause. If the corner wears evenly but the finish is poor, chip load or engagement is the problem. Log the change and keep it with the setup sheet.
Why the same numbers behave differently on two machines
Spindle power and torque curves are not flat. A machine rated at 15 kW may deliver full torque only between 4,000 and 10,000 rpm. Below that range, the control derates the cut. If your calculated rpm sits outside the sweet spot, adjust chip load rather than forcing the spindle.
Structural stiffness sets the chatter threshold. A 4,000 × 400 × 150 mm travel machine has a long cantilever. Push a Ø20 mm tool at the same feed as a compact 500 × 310 × 200 mm machine and the large one will sing. Reduce radial engagement first, then feed. Do not reduce rpm alone; that often makes chatter worse.
Tool holding matters too. A shrink-fit holder runs truer than a worn collet chuck. Runout of 0.02 mm means one tooth does most of the cutting, so effective chip load is higher than you calculated. Check runout with a dial indicator before you blame the numbers.
Thermal drift shows up on long runs. After two hours of roughing, the spindle and ballscrews grow. A feed and speed that held ±0.005 mm at 8 a.m. may drift by mid-afternoon. Re-probe the tool and check the first part of each batch.
Mistakes that cost tools and parts
The most common error is changing rpm to fix chatter. Chatter is a stiffness problem. Lowering rpm may move you away from a resonance, but it also lowers chip load, which increases rubbing and heat. Reduce radial engagement or shorten tool stickout first.
The second is trusting the catalog without checking runout. A collet with 0.03 mm runout loads one flute harder than the others. The tool fails early and the finish shows a pattern. Measure runout at the tool tip, not at the holder.
The third is ignoring the setup sheet. If the operator changes feed and speed on the floor and does not record it, the next run repeats the experiment. A one-line note saves an hour on the next job.
Finally, do not chase maximum removal rate on a finishing pass. Finishing is about surface finish and tolerance. Keep chip load moderate, keep the tool sharp, and let the roughing pass do the heavy work.
Step by step: change feed and speeds on the machine
- 11. Confirm the material and hardnessCheck the cert. 6061-T6 and 6061-O behave differently. 304 and 316L are not the same. If the stock is unknown, cut a test piece first. Hardness above 35 HRC usually means you should reduce surface speed by 30 percent and use a coated grade.
- 22. Pick surface speed for the materialUse the tool maker's chart as a ceiling. Aluminum 6061: 300–500 m/min. 304 stainless: 120–180 m/min. 4140 steel: 90–150 m/min. Ti-6Al-4V: 40–60 m/min. Inconel: 25–35 m/min. Write the number down before touching the control.
- 33. Calculate rpm from diameterrpm = (Vc × 1000) / (π × D). For a Ø10 mm tool in 6061 at 400 m/min, that is about 12,700 rpm. If the spindle cannot reach it, cap rpm at the machine limit and lower chip load instead. Never exceed the tool's rated maximum rpm.
- 44. Set chip load from the chartTypical starting chip load for a Ø10 mm carbide end mill: 0.05–0.08 mm/tooth in aluminum, 0.03–0.05 mm/tooth in steel, 0.02–0.04 mm/tooth in titanium. Multiply by tooth count and rpm to get feed in mm/min. A 3-flute tool at 10,000 rpm and 0.05 mm/tooth gives 1,500 mm/min.
- 55. Reduce for engagement and stickoutLong tool stickout or a thin wall means lower values. If stickout exceeds 4× diameter, cut chip load by 25–40 percent. If radial engagement is under 10 percent, you can raise feed per tooth by 20 percent without overloading the edge.
- 66. Run a single test pass and listenCut one pass in a scrap area or an air-cut with the feed override at 50 percent. Listen for chatter, watch chip color, and check the surface. Aluminum chips should be bright and curl tightly. Blue chips mean too much heat. Fine powder means chip load is too low.
- 77. Step up in small incrementsRaise feed override in 10 percent steps. Stop when chatter appears, then back off 10 percent. Do not change rpm and feed at the same time; you will not know which one caused the change.
- 88. Record the final valuesWrite the rpm, feed, stepover, and depth on the setup sheet. Note the tool, holder, and coolant. The next run starts from a proven point instead of a guess.
Surface speed and chip load by material
Starting values for coated carbide tooling. Reduce by 20–30 percent if the setup is not rigid.
| Material | Surface speed (m/min) | Chip load Ø10 mm (mm/tooth) | Notes |
|---|---|---|---|
| Aluminum 6061 | 300–500 | 0.05–0.08 | Flood coolant, watch for built-up edge |
| Aluminum 7075 | 200–350 | 0.04–0.07 | Harder, less gummy than 6061 |
| Stainless 304 / 316L | 120–180 | 0.03–0.05 | Never rub; keep the edge cutting |
| Steel 4140 | 90–150 | 0.03–0.05 | Reduce speed if hardness exceeds 35 HRC |
| Ti-6Al-4V | 40–60 | 0.02–0.04 | Flood coolant, sharp edges only |
| Inconel | 25–35 | 0.02–0.03 | Low speed, high feed, rigid setup |
| Brass C36000 | 200–400 | 0.05–0.10 | Free-cutting, light coolant |
Symptom, cause, and correction
| Symptom | Likely cause | Correction |
|---|---|---|
| Fine powder chips | Chip load too low | Raise feed per tooth 20 percent |
| Blue or purple chips | Surface speed too high | Lower rpm 15 percent, check coolant |
| Chatter marks | Insufficient rigidity | Reduce radial engagement, then feed |
| Tool breaks on entry | Chip load too high or runout | Check runout, lower feed 25 percent |
| Built-up edge on aluminum | Speed too low or no coolant | Raise rpm, increase coolant flow |
| Rapid corner wear | Abrasive material or hard scale | Use a tougher grade, lower speed |
Frequently asked questions
Should I change rpm or feed first when the cut sounds wrong?
Change feed first. Feed per tooth is the number that controls chip thickness and heat. If the chip looks like powder, raise feed. If the chip is blue, lower rpm.
Only change rpm when the chip color or tool wear points to surface speed. Change one variable at a time so you know what worked.
How do I set feed and speed for a tool with a long stickout?
Start from the chart value, then reduce chip load by 25–40 percent if stickout exceeds 4× diameter. Keep radial engagement light.
If chatter still appears, shorten the stickout before lowering the numbers further. A shorter tool is always stiffer.
Do these values work on a lathe as well as a mill?
The surface speed formula is the same. Feed is expressed per revolution instead of per tooth, so feed = chip load × rpm.
Turning inserts usually run at higher surface speeds than end mills in the same material because the edge is supported by the holder.
What coolant should I use with these numbers?
Aluminum and stainless work well with flood coolant. Titanium needs flood to control heat. Cast iron often runs dry.
If you cut dry, reduce surface speed by 20–30 percent and watch chip color closely.
How do I know the values are right for a finishing pass?
Check the surface finish and the part size. If the finish meets the print and the micrometer reads within tolerance, the values are working.
Do not push removal rate on a finishing pass. Keep the chip load moderate and the tool sharp.
Need parts cut with proven feed and speed data?
Send your drawings. We return a quote and a free DFM analysis within 12 hours, with a process plan that names the material, tool, and cutting values.
12-hour quote100% inspectionNo minimum orderNDA on request
More from the shop floor
We publish setup notes, tooling trials and inspection data from the factory floor.
