SPEEDS AND FEEDS
Every metal cutting operation
requires selection of proper cutting parameters for success. As a DML TA, you need to understand basic
calculations that will allow the tools you use to work as intended.
Example 1A: HSS drill bit (manual)
Example 1B: HSS reamer (manual)
Example 2A: HSS endmill (manual)
Example 2B: Carbide endmill (CNC)
Example 3: Counterbore or countersink (manual)
Example 4: HSS annular cutter (manual)
Example 5: Carbide parting / grooving tool (manual)
Drilling and Milling Speeds and
Feeds Document [RETURN TO QUICK LINKS]
Please begin by reviewing the
comprehensive course document on this topic, as it clearly explains the
process of calculating these parameters for drilling and milling
operations. The governing equations are
summarized below.
N [rpm] = 12 [in/ft] × V
[sfm] / (π × D [in/rev])
Equation (1)
where
N is the rotational velocity of the
tool
V is the recommended peripheral
velocity for the tool being used
D is the diameter of the tool
f [in/min] = N [rpm] × f_{r}
[in/rev] Equation
(2) FOR DRILLING OPERATIONS
f [in/min] = N [rpm] × f_{t}
[in/tooth] × m [# of teeth]
Equation (3) FOR MILLING OPERATIONS
where
f = linear feed rate of the drill /
endmill [in/min]
N = spindle speed [rpm]
f_{r} = feed per revolution
of the drill bit [in/rev]
f_{t} = feed per tooth of the
endmill / cutter [in/tooth]
m = number of teeth on endmill /
cutter [integer]
Recommended
Surface Speeds for Common Materials [RETURN TO QUICK LINKS]
The table below contains a
recommended surface speeds for common materials when using DML equipment. These values are conservative because our
primary goal is fostering a safe learning environment (for our users and our
tools!), not trying to squeeze every second out of each operation.
Material 
Recommended
HSS Speed, V [surface
ft/min] 


Acetal (Delrin) 
250 
Aluminum and its alloys 
250 
Brass (360 high machining) 
250 
Bronze (high tensile) 
100 
Cast Iron (soft) 
100 
Cast Iron (medium hard) 
80 
Cast Iron (hard chilled) 
20 
Hastelloy 
20 
Inconel 
25 
Magnesium and its alloys 
300 
Monel 
25 
High nickel steel 
50 
Mild steel (.2.3 C) 
100 
Steel (.4.5 C) 
60 
Tool steel 
40 
Forgings 
40 
Steel alloys (300400 Brinell) 
30 
Heat Treated Steels 

3540
Rockwell C 
20 
4045
Rockwell C 
20 
4550
Rockwell C 
15 
5055
Rockwell C 
15 
stainless
steel free machining 
40 
stainless
work hardening 
20 
Titanium alloys 
20 


* multiply
surface speeds in table by 2.5 for carbide cutting tools * 

* multiply surface speeds in table by 1.5  2.0
for HEM / HSM toolpaths * 
Recommended Feed Rates for 2 Flute HSS &
Carbide Drills [RETURN TO QUICK LINKS]
Drill Diameter [in] 
Recommended Feed per
Tooth, f_{r} [in/rev] 


Under
1/8” 
Up to 0.002 
1/8”
to 1/4” 
0.002 to 0.004 
1/4”
to 1/2” 
0.004 to 0.008 
1/2”
to 1” 
0.008 to 0.016 
1”
and over 
0.016 and up 


* multiply feed values in table by 0.5
for difficult to machine materials, flexible toolholding or workpieces, or
lighterduty machines* 

*
consult manufacturer’s data for more accurate carbide drill feedrates * 
A general rule of thumb for
materials which are strong enough to support the drilling process is that f_{r}
is between 1  3% of the drill diameter, depending on the material strength.
Recommended Feed Rates for HSS and Carbide
Endmills [RETURN TO QUICK LINKS]
Material 
Recommended Feed per
Tooth, f_{t} [in/tooth] 


Acetal
(Delrin) 
0.008 to 0.030 
Aluminum
and its alloys 
0.004 to 0.012 
Brass
(360 high machining) 
0.004 to 0.012 
Bronze
(high tensile) 
0.002 to 0.006 
Cast
Iron (soft) 
0.002 to 0.006 
Cast
Iron (medium hard) 
0.002 to 0.006 
Cast
Iron (hard chilled) 
0.0015 to 0.004 
Hastelloy 
0.0015 to 0.004 
Inconel 
0.0015 to 0.003 
Magnesium
and its alloys 
0.004 to 0.012 
Monel 
0.0015 to 0.003 
High
nickel steel 
0.002 to 0.004 
Mild
steel (.2.3 C) 
0.002 to 0.008 
Steel
(.4.5 C) 
0.002 to 0.006 
Tool
steel 
0.0015 to 0.004 
Forgings 
0.0015 to 0.004 
Steel
alloys (300400 Brinell) 
0.0015 to 0.004 
Heat
Treated Steels 

3540 Rockwell C 
0.0015 to 0.003 
4045 Rockwell C 
0.0015 to 0.003 
4550 Rockwell C 
0.0015 to 0.003 
5055 Rockwell C 
0.001 to 0.002 
stainless steel (free machining) 
0.002 to 0.006 
stainless steel (work hardening) 
0.0015 to 0.004 
Titanium
alloys 
0.0015 to 0.004 


* table
values are typical for cutters ranging from ½” to 11/2” in size * 
Note there are many other sources
for this data, such as
Machinery Handbook
MariTool
Speeds and Feeds Chart
Harvey
Tool Speeds and Feeds Chart
Melin
Tool Speeds and Feeds Chart
Etcetera
Drill Bit
Speeds and Feeds Calculations (Manual Machine) [RETURN TO QUICK LINKS]
Example 1A: Calculate the
speed and feed for a ¼″ HSS drill bit in mild steel on a manual milling
machine in the lab.
First, lookup the recommended
surface speed in Table 1 (V ≈ 100 ft/min) and calculate the spindle speed from Equation
2:
N [rpm] = 12 × V / (π × D)
= 12 in/ft × 100 ft/min / (π × 0.25
in/rev)
≈ 1500
rpm
Next lookup the recommended feed
per revolution for the drill bit in Table 2
(f_{r} ≈ 0.004 in/rev)
and calculate the feed rate using Equation 3:
f [in/min] = N [rpm] × f_{r} [in/rev]
= 1500 rev/min × 0.004 in/rev
≈ 6.0 in/min
Note that these speed and feed
values are guidelines assuming adequate (flooded) lubrication, workpiece
stiffness and drill depth less than 3 drill diameters (0.75″). When applying oil manually (as in the lab),
scale the feed and speed back to 60%, so N = 900 rpm and f = 3.6 in/min (final answer).
TIP1:
Recommended peck depth when drilling less than 3xD (e.g. 3 drill diameters)
with flooded coolant is one drill diameter, or when applying oil manually, or
under low pressure, is 50% of drill diameter.
TIP2:
When drilling deeper holes (> 3xD) without high pressure TSC (thru spindle
coolant), reduce spindle speed an additional 50%.
Reamer
Speeds and Feeds Calculations (Manual Machine) [RETURN TO QUICK LINKS]
Example 1B: Calculate the
speed and feed for a ¼″ HSS reamer in mild steel on a manual milling
machine in the lab.
TIP: Reamers should
generally be run at half the spindle speed and twice the feed per revolution of
the equivalent sized drill bit.
Based on the previous tip and the
results from Example 1A:
N [rpm] ≈ 0.5 × 1500 rpm ≈ 750 rpm
f [in/min] ≈ 750 rpm × 2 × 0.004 in/rev ≈ 6.0 in/min
Note that these speed and feed
values are guidelines assuming adequate (flooded) lubrication, workpiece
stiffness and drill depth less than 3 drill diameters (0.75″). When applying oil manually (as in the lab),
scale the feed and speed back to 60%, so N = 450 rpm and f = 3.6 in/min (final answer).
Endmill
Speeds and Feeds Calculations (Manual Machine) [RETURN TO QUICK LINKS]
Example 2A: Calculate the
speed and feed for a 1″ diameter, 4 flute HSS endmill in aluminum using a
manual milling machine in lab.
First, lookup the recommended
surface speed in Table 1 (V ≈ 250 ft/min) and calculate the spindle speed from Equation
2:
N [rpm] = 12 × V / (π × D)
= 12 in/ft × 250 ft/min / (π × 1
in/rev)
≈ 950
rpm
Next, lookup the recommended feed
per tooth (chipload) in Table 3 (f_{t} ≈ 0.008 in/tooth)
and calculate the feed rate using Equation 3:
f [in/min] = N [rpm] × f_{t} [in/rev]
× m
= 950 rev/min × 0.008 in/tooth × 4
teeth/rev
≈ 30 in/min
Note that these speed and feed values
are guidelines assuming proper (flooded) lubrication, workpiece stiffness and
depth of cut. When applying oil manually
(as in the lab), scale the feed and speed back to 60%, so N = 570 rpm and f ≈ 18 in/min (final answer). Note also this problem assumes we peripheral
milling versus plunge milling (since we never teach the students the latter in
lab).
Endmill
Speeds and Feeds Calculations (CNC Machine)
[RETURN TO QUICK LINKS]
Example 2B: Calculate the
speed and feed for a 1/2″ diameter, 3 flute carbide endmill if peripheral
and plunge cutting in aluminum using a CNC milling machine in lab.
First, lookup the recommended
surface speed in Table 1 (V ≈ 625 ft/min) and calculate the spindle speed from Equation
2:
N_{peripheral} [rpm] = 12 × V /
(π × D)
= 12 in/ft × 625 ft/min / (π × 0.5
in/rev)
≈
4700 rpm
Next, lookup the recommended feed
per tooth (chipload) in Table 3 (f_{t} ≈ 0.004 in/tooth)
and calculate the feed rate using Equation 3:
f_{peripheral} [in/min] = N [rpm] × f_{t}
[in/rev] × m
= 4700 rev/min × 0.004 in/tooth × 3 teeth/rev
≈ 56 in/min
TIP: Plunging should
generally be performed at 75% of the speed and 25% of the feedrate of the
calculated peripheral cutting parameters.
Based on the previous tip,
calculate the same parameters for plunge milling using the noted scaling
factors:
N_{plunge} ≈ 0.75 × N_{peripheral}
≈ 0.75 × 4700 rpm
≈ 3525 rpm
f_{plunge} ≈ 0.25 × f_{peripheral}
≈ 0.25 × 56 in/min
≈ 14 in/min
Note that these speed and feed
values are guidelines assuming proper (flooded) lubrication, workpiece
stiffness and depth of cut. When
learning how to use the CNC, always start lower (around 60% on the spindle
speed and feedrate override buttons) and work your way up as you gain
confidence or purchase your own tools (lol).
Countersink Speeds and Feeds
Calculations (Manual Machine) [RETURN TO
QUICK LINKS]
Example 3: Calculate the
speed and feed for a HSS countersink used to countersink a #10 clearance hole
in aluminum using a manual milling machine.
TIP: Countersinking
should generally be performed at 25% of the speed and the same feed per
revolution as the equivalent sized drill.
First, lookup the recommended
surface speed in Table 1 (V ≈ 250 ft/min) and calculate the spindle speed from Equation
2:
N [rpm] = 12 × V / (π × D)
= 12 in/ft × (0.25 × 250) ft/min / (π × 0.42 in/rev) (the largest part of the countersink measures 0.42” in diameter)
≈ 550
rpm
Next lookup the recommended feed
per revolution for the equivalent size drill bit in Table 2 (f_{r}
≈ 0.006 in/rev) and calculate the feed rate using Equation 3:
f [in/min] = N [rpm] × f_{r} [in/rev]
= 550 rev/min × 0.006 in/rev
≈ 3.3 in/min
Note that these speed and feed
values are guidelines assuming adequate (flooded) lubrication and workpiece
stiffness. When applying oil manually
(as in the lab), scale the feed and speed back to 60%, so N = 330 rpm and f = 2.0 in/min (final answer).
Annular Cutter Speeds and Feeds Calculations (Manual Machine) [RETURN TO
QUICK LINKS]
Example 4: Calculate the
speed and feed for a 1″ diameter, 6 flute HSS annular cutter in ¼” thick
aluminum on a manual milling machine in the lab.
TIP1: Since annular
cutting is a plunging operation, it should generally be performed at 75% of the
speed and 25% of the feedrate of the calculated peripheral cutting parameters
(as with endmill plunging).
TIP2: Do not plunge
an annular cutter at a feedrate less than 0.001 ipt (inch per tooth) in strain
hardening materials like 304 stainless or titanium.
First, lookup the recommended
surface speed in Table 1 for a 1” HSS endmill
cutting aluminum (V ≈ 250
ft/min) and calculate the spindle speed from Equation 2 using the
aforementioned 75% speed reduction:
N [rpm] = 12 × V / (π × D)
= 12 in/ft × (0.75 × 250) ft/min / (π × 1 in/rev)
≈ 700
rpm
Next, calculate the feed rate
used for plunging. Remember annular cutters
should be fed at approximately 25% of the feedrate for an equivalent sized
endmill. From Table 3, lookup the recommended feed per tooth
for a 1″ HSS endmill (f_{t}
≈ 0.008 in/tooth) and calculate the plunge feed rate using Equation 3:
f [in/min] = N [rpm] × f_{r} [in/rev]
= 700 rev/min × (0.25 × 0.008) in/tooth
x 6 teeth/rev
≈ 8 in/min
Note: when applying oil manually,
scale the feed and speed back to 60%, so N ≈ 420 rpm and f ≈ 4.8 in/min (final answer). This is close enough to 500 rpm that I would
first try this tool at the low end of high range with good oil application and
see how it goes.
Lathe Partoff
Operation Speed Calculation (Manual Machine)
[RETURN TO QUICK LINKS]
Example 5: Calculate the speeds
for parting off 1” diameter aluminum and 1” diameter mild steel workpieces on
the lathe using the standard carbide partoff inserts.
First, lookup the recommended
surface speeds in Table 1 (V_{ALUM} ≈ 625 ft/min, V_{STEEL} ≈ 250 ft/min (notice the 2.5 multiplier))
Next, calculate the spindle
speeds from Equation 2:
N_{ALUM} [rpm] = 12 × V_{ALUM}
/ (π × D)
= 12 in/ft × 625 ft/min / (π × 1 in/rev)
≈ 2375 rpm
N_{STEEL} [rpm] = 12 × V_{STEEL}
/ (π × D)
= 12 in/ft × 250
ft/min / (π × 1 in/rev)
≈ 950 rpm
Note: since applying oil
manually, scale the speeds back to 60%, so N_{ALUM} ≈ 1425 rpm
and N_{STEEL} ≈ 570 rpm
(final answer). Note these are
MAXIMUM values and lathe chuck safety must take precedence; spinning the lathe
chuck at 570 rpm is about the upper limit of what we safely do in the lab, so for smaller or easier to machine workpieces, DO NOT EXCEED
600 RPM regardless of the calculation results, unless you are running a collet
chuck.
TIP:
IF this was being performed on a CNC lathe, typical parting feed rates vary
between 0.001 in/rev (for steels) and 0.005 in/rev (for plastics). But remember, do NOT use the power feed when
parting on a manual lathe unless you own the machine!
Notes on Plastics [RETURN TO
QUICK LINKS]
As shown in the following chart,
plastics vary widely in regards to their machinability.
As you can see Acetal (Delrin) is
one of the most machinable plastics and nylon is four times less machinable
(which is why it should usually be avoided!).
TIP:
When working with plastics with good machinability, use the cutting parameters
for aluminum up until the point that the plastic melts.
Here are some tips on selecting
plastics for machinability.