Technical Resources

Click on tabs below to navigate our resources. Need more help? Please CONTACT US
Speeds & FeedsSpeeds & Feeds - CarbideClimb MillingDrill Time FormulaTool Coatings

Speeds & Feeds

Modern milling cutters capable of operating at higher feeds and speeds, and moving more cubic inches of metal per minute, require greater machine rigidity and more power.
Therefore it is important to determine that enough power is available to handle the desired depth and width of cut at the higher feeds and speeds.

T= Number of teeth in cutter
D= Cutter diameter in inches
RPM= Revolutions per minute
SFM= Surface feet per minute
F= Feed in inches per minute

f= Feed per tooth in inches
W= Width of cut
d= Depth of cut
HP= Motor horsepower
C= Machinability constant

Machinability constant values for various materials are based on removing one cubic inch of metal per minute per horsepower with 60% power efficiency at the spindle nose and a 25% allowance for cutter dulling.
Aluminum, Magnesium, Dural – 4.0 plus
Brass – 2.5
Soft Bronze, Copper – 2.0
Cast Iron – 1.5
Steel up to 150 Brinell, Malleable Iron – 0.75
Steel, 300 Brinell, Hard Bronze – 0.6
Steel, 400 Brinell – 0.5

Speeds & Feeds – Carbide

Climb Milling

In conventional milling, the cutter revolves opposite to the direction of table feed. Therefore the width of the chip starts at zero and increases to a maximum at the end of the cut. This can lead to accelerated tool wear under some conditions – conventional milling is recommended for hot rolled steel, surface hardened materials and steels with a surface scale. In climb milling, the cutter revolves in the same direction as the table feed. The tooth meets the work at the top of the cut, producing the thickest part of the chip first. In horizontal applications the resultant force created by climb milling can act as a clamping force, acting toward the machine table. It is important to make sure that the machine tool has no leadscrew backlash. Normally climb milling improves product surface finish and increases tool life.

Advantages of Climb Milling

Longer Tool Life: Since the chips produced are deposited behind the cutter, tool life can be substantially increased.

Ease of Fixturing: Climb milling exerts a downward clamping force on the workpiece and not an upward force as in conventional milling, which results in simplified fixturing.

Improved Surface Finish: Since the chips are not carried by the cutter, less likelihood of marring the machined surface.

Lower Power Requirements: A higher rake angle can be utilized, lowering power consumption.

Better Chip Evacuation: Easier and faster chip removal since chips are deposited behind the cutter.

Drill Time Formula

Speeds & Feeds – Formula

Find: Have: Formula:
Revolutions per minute (RPM) SFM (SFM x 12) / (Diameter of drill x 3.1416)
Surface feet per minute (SFM) RPM (Diameter of drill x RPM x 3.1416) / 12
Feed rate per RPM (FR) SFM and FM (Diameter of drill x FM x 3.1416) / (SFM x 12)
Feed rate per RPM (FR) RPM and FM FM / RPM
Feed rate per minute (FM) FR and RPM RPM x FR
SFM RPM and drill dia. .26 x RPM x drill diameter
RPM SFM and drill dia. 3.8 x (SFM / drill diameter)

Drill Speeds

Material SFM*
Aluminum and Aluminum Alloys 150-300
Brass and Bronze (free cutting) 150-300
Brass and Bronze (high tensile) 70-120
Cast Iron (soft) 80-120
Cast Iron (medium) 60-90
Cast Iron (hard) 30-70
Copper 70-100
Magnesium 200-400
Nickel Base Alloys 20-50
Plastic and Related Materials 100-200
Wood 200-300

*Surface feet per minute

Drilling Time Formula

Time (Minutes) = Travel(in.) / RPM x Feed (per rev.)

Travel = Sum of: Depth of Hole, 1/3 Drill Diameter, Approach Clearance, Over Travel (through cavities) / Total Travel (in.)

Drill Speeds (Steel)

Material SFM*
Alloyed – under 200 B.H. 60-90
Alloyed – 200 – 300 B.H. 40-70
Alloyed – over 300 B.H. 20-30
Cast and Forged 40-70
Heat Treated – 35 – 40 R.C. 30-40
Heat Treated – 40 – 45 R.C. 20-30
Heat Treated – over 45 R.C. 10-20
Mild – .2 – .3 Carbon 70-100
Mild – .4 – .5 Carbon 50-80
Stainless – 300 Series 20-50
Stainless – 400 Series 30-70
Tool – over 1.0 Carbon 40-60
Titanium Alloys 20-50

*Surface feet per minute

Drill Feeds

Diameter (in.) Light Feeds Heavy Feeds
1/8 .0005 – .0010 .0015
3/16 .0010 – .0015 .0020
1/4 .0015 – .0020 .0025
5/16 .0020 – .0025 .0030
7/16 .0025 – .0030 .0035
1/2 .0035 – .0040 .0045
5/8 .0045 – .0050 .0055
3/4 .0055 – .0060 .0065

The above are suggested ranges. Due to many variable in an operation, more optimum speed may be established through trial.

Tool Coatings

TiN – General purpose coating for Steels, Stainless Steels and Inconel. Excellent wear characteristics in roughing applications.

TiCN – High performance in Die and Mold Steels, Hardened Materials, Steels and Stainless Steel. Ability to run at increased Feeds and Speeds over TiN coated tools.

TiALN – Best results in Dry Milling applications at high temperatures. Works well in Hardened Materials, Titanium Alloys, Stainless Steels, Cast Irons, Graphite and HSM applications.