Setting Speeds & Feeds
Most tooling that wears out early, breaks or leaves a poor finish was run at the wrong speed or feed. This guide shows how to turn the figures in our charts into machine settings, and how to tell from the sound and the chips whether they are right.
Cutting speeds, feeds & insert chart
Cutting speed and rpm
The cutting speed (Vc, in metres per minute) is how fast the cutting edge moves over the work. It depends on the material you are cutting and the tool material - roughly, carbide runs several times faster than HSS, aluminium and brass can be cut much faster than steel, and stainless and tool steels need to be cut slower. Take the figure from the cutting speeds chart.
The rpm then depends on the diameter - a big drill or cutter needs fewer rpm than a small one for the same cutting speed:
rpm = Vc × 1000 ÷ (3.14 × diameter in mm)
or near enough: rpm = Vc × 318 ÷ diameter
Example: a 10 mm HSS drill in mild steel at 25 m/min: 25 × 318 ÷ 10 = about 800 rpm. The same drill at 30 mm diameter would want only about 265 rpm.
On a geared machine, pick the nearest speed below the figure. For turning, the diameter is the work, not the tool - so the rpm goes up as you turn or face down to a smaller diameter.
Feed
Drilling and turning - the feed is in mm per revolution, and it comes from the chart by drill size or insert. On a drill with a power feed, set it directly; by hand, aim for a steady chip, not dust and not a struggle.
Milling - the chart gives the feed per tooth (fz). The table feed is:
feed (mm/min) = fz × number of flutes × rpm
Example: a 10 mm four-flute HSS end mill at 0.03 mm per tooth and 800 rpm: 0.03 × 4 × 800 = about 96 mm/min.
For light side cuts - less than about a quarter of the cutter diameter - the chip is thinner than the feed per tooth suggests, so the feed can go up. The chart covers this under chip thinning.
Listen and look at the chips
The figures are a starting point. The machine, the setup and the coolant all change what works, so adjust from what you see and hear:
| What you see or hear | What it usually means |
|---|---|
| Screeching or squealing | Speed too high, or the feed too light so the tool rubs |
| Chatter - a rattling noise and a wavy finish | Something not rigid - too much overhang, a loose setup or worn bearings; try lower rpm and a heavier feed |
| Blue or smoking chips from an HSS tool | Too fast or too little coolant - the tool is about to burn |
| Fine dust or powder instead of chips | Feed too light - the tool is rubbing. Bad on stainless, which work-hardens; keep the feed up |
| Long stringy chips that wrap round the tool | Feed too light for the chipbreaker, or no chipbreaker - increase the feed or peck |
| Short, tightly curled chips shaped like a 6 or a 9 - "sixes and nines" | About right |
Aim for sixes and nines. When turning or drilling steel, a good chip curls round once or twice and breaks off in a short coil that looks like the figure 6 or 9. It carries the heat away from the tool and clears itself from the cut. Long ribbons mean the chip is not breaking; dust or tiny flakes mean the tool is rubbing rather than cutting.
Other materials behave differently. Cast iron and brass naturally break into small granules or flakes, so a powdery chip there is normal. Aluminium tends to form longer, shinier curls and can weld onto the cutting edge if the speed or coolant is wrong. Stainless steel, copper and plastics each have their own habits - judge them against what a sharp tool at the chart settings produces.
If you change something, change one thing at a time.
Coolant and cutting fluid
- Steel and stainless - use cutting fluid or soluble oil, especially for drilling, tapping and reaming.
- Cast iron and brass - usually cut dry; cast iron dust and coolant make a paste.
- Aluminium - use a fluid made for non-ferrous metals to stop it sticking to the cutting edge.
- Flood coolant beats a drip - a little coolant on hot carbide can crack it, so with carbide either flood it or run dry.
DORMER M200 non-ferrous cutting fluidTachometer - check the real rpm
Tooling
Drills and holemakingMilling cuttersTurning inserts and holdersDORMER A100 jobber drills
Still not sure? Bring it in or ask us - we are happy to help.