Current site:
Current language:
Unit of measurement:
Please select your country!


{{"ifind_go-back" | translate}}


General face milling


​What is face milling?

Face milling is the most common milling operation and can be performed using a wide range of different tools. Cutters with a 45º entering angle are most frequently used, but round insert cutters, square shoulder cutters and side and face mills are also used for certain conditions.


Choice of tools

​Overview of face milling cutters

The diagram below shows the main application area for different cutter concepts, in terms depth of cut, ap, and feed per tooth, fz.



Direction of cutting forces generated by different entering angles.



  • First choice for general purpose
  • Reduce vibrations on long overhangs
  • Chip thinning effect allows increased productivity


​90° cutters

  • Thin walled components
  • Weak-fixtured components
  • Where 90° form is required



​Round insert cutters

  • General purpose cutter
  • Strongest cutting edge
  • Many edges per insert
  • Especially suitable for heat-resistant alloys, ISO S.
  • Smooth cutting action


Application checklist and hints

​Roll into cut
  • Consider machine tool stability, spindle size and type (vertical or horizontal) and available power.
  • Use a cutter diameter that is 20 to 50% larger than the workpiece.
  • Consider maximum chip thickness when positioning the cutter for optimum feed.
  • Position the cutter off centre to produce the thinnest chip at exit.
  • Apply down-milling for favourable chip formation, i.e. thick to thin chip.
  • Program the cutter to roll into the cut and reduce the feed to obtain a smooth entry.


​Keep cutter constantly engaged.
  • Apply down-milling for favourable chip formation, i.e. thick to thin chip.​
  • Avoid entries and exits through tool path programming.
  • Frequent entering and exiting the workpiece should be avoided if possible. It can create unfavorable stresses on the cutting edge, or cause dwell and chatter tendencies. It is recommended that you program a tool path that keeps the milling cutter in full contact, rather than performing several parallel passes. When changing direction, include a small radial tool path to keep the cutter moving and constantly engaged.


How to apply

​Intermittent face milling of surfaces with interruptions


​Avoid milling over interruptions
  • If possible, avoid milling over interruptions (holes or slots). Such intermittent cuts are demanding on the cutting edges as they cause multiple entries and exits.
  • Alternately, reduce the recommended feed rate by 50% over the workpiece area that contains the interruptions.


Face milling of thin-walled and deflecting sections


  • Consider the direction of the main cutting forces in relation to the stability of the workpiece and the fixture.
  • When milling axially-weak components, use a 90° shoulder milling cutter, as it directs the major portion of the cutting forces in an axial direction.
  • Alternately, use a light-cutting, face milling cutter.
  • Avoid axial depths of cut that are smaller than 0.5–2 mm to minimize axial forces.
  • Use a coarse-pitched cutter to obtain the smallest possible number of edges in cut.
  • Use sharp, positive (-L) edges to minimize cutting forces.


Edging of thin sections using face milling cutters


  • The cutter should be positioned off centre for face milling operations on the edges of thin sections. The cut becomes smoother and the cutting forces are directed more uniformly along the wall, which reduces the risk of vibration.
  • Select a cutter pitch for these operations that maintains more than one insert in the cut at all times.
  • Use the lightest insert geometry possible (light instead of medium, or medium instead of heavy).
  • Select a smaller insert radius and shorter parallel land to lower the risk of vibration in thin-walled components.
  • Use low cutting data, small cutting depth, ap, and low feed/tooth, fz.


We use cookies to enhance the experience on our website. More about cookies.