Please select your country! -English -EN Settings


Please select your country!


{{"ifind_go-back" | translate}}



Drilling tips

​Coolant supply tips and tricks

Having a correct coolant supply is crucial in order to achieve successful performance in drilling. The coolant supply influences:

  • Chip evacuation
  • Hole quality
  • Tool life

The coolant tank volume should be between 5-10 times larger than the volume of coolant that the pump supplies per minute. It is important to have sufficient coolant flow.

The volume capacity can be checked using a stop-watch and a suitably sized bucket.

Pressure-diameter relationship in cutting fluid supply
(pressure in red, diameter in yellow, volume in blue)​

Check the volume coming out from the drill​
  • Soluble oil (emulsion) should always be used with EP (extreme pressure) additives. The mixture of oil and water should be between 5-12% oil for best tool life (10-15% for stainless steels and heat resistant alloy materials). When increasing percentage of oil in cutting fluid, always check with the oil distributor to be sure to not exceed recommended percentages of oil
  • Internal coolant supply is always favourable, when applicable, as compared to externally applied
  • Neat oil improves lubrication and is beneficial when drilling stainless steels. Always use with EP additives. Both solid carbide drills and indexable insert drills work well with neat oil
  • Compressed air, mist cutting fluid or MQL (Minimum Quantity Lubrication) can be successful under favourable conditions, especially for some cast irons and aluminium. Reduced cutting speed is recommended due to elevated temperatures which in turn can negatively impact tool life
​Internal coolant

Internal coolant is always preferred to avoid chip jamming, especially in long chipping materials and when drilling deeper holes (>3 x DC).

A horizontal drill should have a flow of coolant coming out of the drill without any downward drop for at least 30 cm (11.81 inch).

​External coolant

External coolant supply can be used when chip formation is good and when hole depth is shallow. To improve chip evacuation, at least one coolant nozzle (two if drill is stationary) should be directed closely to the tool axis.

Dry drilling tips, without coolant

Dry drilling is generally not recommended.

  • Can be used for short-chipping materials at hole depths up to 3 times the diameter
  • Preferably in horizontal applications
  • Reduced cutting speed is recommended
  • Tool life will be reduced

It is never recommended to use dry drilling for:

  • Stainless materials (ISO M and S)
  • Exchangeable-tip drills
High pressure coolant (HPC) (~70 bar)

The benefits to using high pressure coolant are:

  • Longer tool life due to improved cooling effect
  • Improved chip evacuation and possibly tool life in long-chipping materials such as stainless steels
  • Improved security due to better chip evacuation
  • Provides sufficient flow for a given pressure and hole size to maintain delivery

​Chip control tips

Chip formation and chip evacuation are critical issues in drilling and depend on the workpiece material, choice of drillI/insert geometry, coolant pressure/volume, cutting data.

Chip jamming can cause radial movement of the drill and consequently affect hole quality, drill life and reliability, or drill/insert breakages.

Thicker and stiffer chips​
Speed​ More open due to less friction​

Chip formation is acceptable when the chips can be evacuated from the drill without disturbance. The best way to identify this is to listen during drilling. A consistent sound means that chip evacuation is good, but an interrupted sound indicates chip jamming. Check the feed force or power monitor. If there are irregularities, chip jamming can be the reason. Look at the chips. If they are long and bent, instead of curled, chip jamming has occurred. Look at the hole. If chip jamming has occurred, an uneven surface will be visible.

A hole with good chip evacuation

A hole affected by chip jamming


Tips to avoid chip jamming:

  • Make sure the right cutting data and drill/tip geometry is used
  • Inspect chip form – adjust feed and speed
  • Check the cutting fluid flow and pressure
  • Inspect the cutting edges. Long chips can be caused by damages/chipping on the cutting edge when the entire chip breaker is not engaged
  • Check if machinability has changed due to new workpiece batch – adjust cutting data

​Excellent, acceptable and unacceptable chips

​Indexable insert drills

The central insert forms a conical chip that is easy to identify. The peripheral insert forms a chip similar to that formed by turning.

Central strip Peripheral chip​
Excellent​ Excellent​
Acceptable​ Acceptable​
Chip jamming​ Chip jamming​
​Solid carbide drills

One chip is formed from the centre to the periphery of the edge.

Chip jamming
Start chip

Note: The start chip from entering into the workpiece is always long and does not create any problems.

​Exchangeable-tip drills



Unacceptable, risk for chip jamming


Tips and tricks for feeds and speeds

vc (m/min)
fn (mm/r)
​​Effects of cutting speed – vc (m/min(ft/min))

Cutting speed is the main factor, along with material hardness, that affects tool life and power consumption.

  • Cutting speed is the largest factor determining tool life
  • Cutting speed affects the power Pc (kW) and torque Mc (Nm)
  • Higher speed generates higher temperature and increased flank wear, especially on the peripheral corner
  • Higher speed is beneficial for chip formation in certain soft, long-chipping materials, i.e. low carbon steel
  • Too high cutting speed:
    • Rapid flank wear
    • Plastic deformation
    • Poor hole quality and bad hole tolerance
  • Too low cutting speed:
    • Built-up edge
    • Bad chip evacuation
    • Longer time in cut
​​Effects of feed – fn (mm/r(in/r))
  • Influences chip formation, surface finish and hole quality
  • Affects the power Pc (kW) and torque Mc (Nm)
  • High feed affects the feed force Ff (N), to be considered when conditions are unstable
  • Contributes to mechanical and thermal stress
  • High feed rate:
    • Harder chip breaking
    • Less time in cut
    • Less tool wear but increased risk for drill breakages
    • Reduced hole quality
  • Low feed rate:
    • Longer, thinner chips
    • Quality improvement
    • Accelerated tool wear
    • Longer time in cut

When drilling a thin/weak component, the feed rate should be kept low.


Tips for achieving good hole quality

  • Chip evacuation
  • Make sure chip evacuation is satisfactory. Chip jamming affects hole quality and reliability/tool life. Drill/insert geometry and cutting data are crucial.

  • Stability, tool set-up
  • Use the shortest possible drill. Use a rigid and accurate tool holder with minimum run-out. Make sure the machine spindle is in good condition and is well-aligned. Ensure component is fixed and stable. Establish correct feed rates for irregular, angular surfaces and cross holes.

  • Tool life
  • Check insert wear and establish pre-determined tool life program. The most effective way to supervise drilling is by using a feed force monitor.

  • Maintenance
  • Change insert-clamping screw regularly. Clean the tip seat before changing insert and make sure to use a torque wrench. Don’t exceed maximum wear before regrinding solid carbide drills.


Drilling tips and techniques for different materials

  • Low carbon steel
  • Austenitic and duplex stainless steels
  • CGI (Compact Graphite Iron)
  • Aluminium alloys
  • Titanium and Heat Resistant Alloys
  • Hard steels

Drilling low carbon steel tips

Issue: Chip formation can be a difficult issue with low carbon steels, which often are used for welded components. The lower the hardness, carbon and sulphur content of the steel, the longer the chips are that will be produced.

Recommendations: If problems with chip formation occur, increase the speed, vc, and decrease the feed, fn (note in normal steels, the feed should be increased).

Other: Use high pressure and internal coolant supply.

Drilling austenitic and duplex stainless steel tips

Issue: Austenitic, duplex, and super duplex materials can cause problems with chip formation and evacuation.

Recommendations: The correct geometry is crucial as it enables chips to form properly and aids their evacuation. In general terms, a sharp cutting edge is preferable. If problems with chip formation occur, increasing the feed, fn will allow the chips to break more easily.

Other: Internal coolant, high pressure.

Drilling CGI (Compact Graphite Iron) tips

Issue: CGI does not normally require extra attention. It produces larger chips than grey cast iron, but they are well broken. Cutting forces are higher, which affects tool life. Extra wear resistant grades are necessary. Corner wear is typical as in all cast irons.

Recommendations: If problems with chip formation occur, increase the speed, vc, and decrease the feed, fn.

Other: Internal coolant.

Drilling aluminium alloy tips

Issue: Burr formation and chip evacuation can be a problem. Poor tool life can also be present due to adhesion.

Recommendations: For best chip formation, use low feed and high speed.

In order to avoid poor tool life it may be necessary to test different coatings, minimizing adhesion. These coatings could include diamond coatings or certain cases (depending on the substrate) not using any coating at all.

Other: Use emulsion or mist coolant at high pressure.

Drilling titanium and Heat Resistant Alloy tips

Issue: Work hardening of hole surface affects subsequent operations. Good chip evacuation can be difficult to obtain.

Recommendations: When selecting a geometry for titanium alloys it is preferable to have a sharp cutting edge. For Nickle-based alloys, having a robust geometry is crucial. If work hardening is an issue, attempt to increase feed rate.

Other: High pressure (up to 70 bar) coolant improves performance.

Drilling hard steel tips

​Issue: Obtaining an acceptable tool life.

Recommendations: Lower cutting speed in order to reduce heat. Adjust feed rate in order to obtain acceptable chips that can be easily evacuated.

Other: Emulsion with a high mixture.


Hole tolerance tips

The dimensions of a hole can be divided into three parameters:

  • The nominal value (the theoretically exact value)
  • The tolerance width (designated IT acc. to ISO)
  • The position of the tolerance (designated by capital letters acc. to ISO)

Dmax minus Dmin is the tolerance width also called IT.

Diameter range, D (mm)
​Tool width​D>3-6​​D>6-10​D>10-18​D>18-30​D>30-50​D>50-80​D>80-120​D>120-180​D>180-250
Diameter range, D (inch)
​Tool width​D>0.118-0.236​​D>0.236-0.394​D>0.394-0.709​D>0.709-1.181​D>1.181-1.969​D>1.969-3.150​D>3.150-4.724​D>4.724-7.087​D>7.0879.843
​​IT120.00470.0059 0.00710.00830.00980.01180.01380.01570.0181
  • The lower the IT-number, the closer the tolerance
  • The tolerance for one IT class increases at larger diameters
One example:
Nominal value: 15.00 mm
Tolerance width: 0.07 mm (IT 10 acc. to ISO)
Position: 0 to plus (H acc. to ISO)

​Hole and axle tolerances

The hole tolerance is often connected to the tolerance of an axle that should fit the hole.

Axle ø20 mm (0.787 inch) h7​Hole ø20 mm (0.787 inch) h7​

Axle tolerance position is designated by lower case letters that correspond to the hole tolerances. The figure below provides a complete picture:

Most common​
Hole larger
than axle​
Axle larger
than hole​
Running fit | Slide fit​Drive fit | ​Interference​
Play (bearings) Grip (=negative play (fixed joints)​
We use cookies to enhance the experience on our website. More about cookies.