Please select your country! -English (US) -EN Settings


Please select your country!


{{"ifind_go-back" | translate}}



Milling troubleshooting

Milling troubleshooting tips about vibration issues, chip jamming, re-cutting of chips, unsatisfactory surface finish, burr formation, machine power and tool wear are presented in the following table.

Cause Solution


  • Weak fixture
  • Assess the direction of the cutting forces and provide adequate support or improve the fixture
  • Reduce the cutting forces by decreasing the cutting depth, ap
  • Select a coarse and differentially pitched cutter with a more positive cutting action
  • Select a geometry with a small corner radius and small parallel land
  • Select a fine-grain, uncoated insert, or a thinner coating
  • Avoid machining where the workpiece has poor support against the cutting forces
  • Axially weak workpiece
  • Consider a square shoulder cutter (90-degree entering angle) with positive geometry
  • Select an insert with L-geometry
  • Decrease axial cutting force – use a lower depth of cut, smaller corner radius and parallel land
  • Select a coarse-pitch cutter with differential pitch
  • Check tool wear
  • Check tool holder run-out
  • Improve the clamping of tools
  • Tool overhang too long
  • Minimize overhang
  • Use coarse-pitch cutters with differential pitch
  • Balance radial and axial cutting forces – use a 45-degree entering angle, large corner radius or round insert cutter
  • Increase feed per tooth
  • Use a light-cutting insert geometry
  • Reduce axial depth of cut, af
  • Use up milling in finishing
  • Use oversized cutters and Coromant Capto® coupling adapters
  • For solid carbide end mills and exchangeable-head mills, try a tool with fewer teeth and/or a higher helix angle
  • Milling a square shoulder with a weak spindle
  • Select the smallest possible cutter diameter​
  • ​Select a positive and light-cutting cutter and insert
  • ​Try up milling
  • ​Check spindle deflection to see if it is acceptable for the machine
  • Irregular table feed
  • Try up milling​
  • ​Tighten the machine feed mechanism: adjust the feed screw on CNC machines
  • Adjust the locking screw or replace the ball screw on conventional machines​
  • Cutting data
  • Reduce cutting speed, vc
  • Increase feed, fz
  • Change the cutting depth, ap
  • Bad stability
  • Reduce overhang
  • Improve stability
  • Vibration in corners
  • Program large corner radii with a reduced feed rate

Chip jamming
A common obstacle when full slotting –
especially in long-chipping materials​​
  • Insert corner damage
  • Edge chipping and breakage
  • Re-cutting of chips
  • Improve chip evacuation by using rich and well-directed cutting fluid or compressed air
  • Reduce feed, fz
  • Split deep cuts into several passes
  • Try up milling in deep slotting
  • Use coarse pitch cutters
  • Use solid carbide end mills or exchangeable-head mills with two or a maximum of three cutting edges and/or a higher helix angle

Re-cutting of chips
Appears in full slotting and pocketing –
especially in titanium. Also common when milling deep cavities and pockets on vertical machines.​​
  • Cutting edge fractures
  • Harmful for tool life and security
  • Chip jamming
  • Evacuate chips effectively with compressed air or copious cutting fluid flow – preferably internal coolant
  • Change the cutter position and tool path strategy
  • Reduce feed, fz
  • Split deep cuts into several passes

Unsatisfactory surface finish​​
  • Excessive feed per revolution
  • Set cutter axially or classify inserts. Check height with indicator
  • Check spindle run-out and cutter mounting surfaces
  • Decrease feed per rev to max 70% of the width of the parallel land
  • Use wiper inserts if possible (for finishing operations)
  • Vibration
See “Vibration” section above
  • Built-up edge formation
  • Increase cutting speed, vc, to elevate machining temperature
  • Turn off cutting fluid
  • Use sharp cutting edge inserts with a smooth rake side
  • Use positive insert geometry
  • Try a cermet grade with higher cutting data
  • Back-cutting
  • Check spindle tilt (approx. 0.10 mm/1,000 mm (0.004 inch/39.370 inch))
  • Axial run-out, TIR, of spindle should not exceed 7 microns during finishing
  • Reduce the radial cutting forces (decrease the depth of cut, ap)
  • Select a smaller cutter diameter
  • Check the parallelism on the parallel lands and on the wiper insert used (should not be standing on “heel or toe”)
  • Make sure the cutter is not wobbling – adjust the mounting surfaces
  • Workpiece frittering
  • Decrease feed, fz
  • Select a close or extra-close pitch cutter
  • Re-position the cutter for a thinner chip at exit
  • Select a more suitable entering angle (45 degrees) and lighter cutting geometry
  • Choose a sharp insert
  • Monitor flank wear to avoid excessive wear

Burr formation
  • Material-specific – HRSA/stainless steel
  • Notch on main wear mechanism
  • Use a large radius with a low insert entry angle
  • Keep the depth of cut below the radius
  • ap = 0.5 x radius​

Machine power
Be aware of the power curve, as the machine may lose efficiency if the rpm is too low.
The power requirements in milling vary with the:
  • Amount of metal to be removed
  • Average chip thickness
  • Cutter geometry
  • Cutter speed
  • Go from close to coarse pitch, i.e. fewer teeth
  • A positive cutter is more power-efficient than a negative cutter
  • Reduce cutting speed before table feed
  • Use a smaller cutter and make several passes
  • Reduce depth of cut, ap

Insert wear

To achieve optimized cutting data and the best possible component quality and tool life, always remember to check the insert/cutting edge after machining. Use this list of causes and solutions for different forms of insert wear as a reference for successful milling.

Cause Solution

Flank wear
Rapid wear results in a poor surface finish or being out of tolerance.
  • Cutting speed too high
  • Insufficient wear resistance
  • Feed, fz, too low
  • Reduce cutting speed, vc
  • Select a more wear-resistant grade
  • Increase feed, fz

Flank wear
Excessive wear results in short tool life.
  • Vibration
  • Re-cutting of chips
  • Burr formation on component
  • Poor surface finish
  • Heat generation
  • Excessive noise
  • Increase feed, fz
  • Use down milling
  • Evacuate chips effectively using compressed air
  • Check recommended cutting data

Flank wear
Uneven wear causes corner damage.
  • Tool run-out
  • Vibration
  • Short tool life
  • Bad surface finish
  • High noise level
  • Radial forces too high
  • Reduce run-out to below 0.02 mm (0.0008 inch)
  • Check chuck and collet
  • Minimize tool protrusion
  • Use fewer teeth in cut
  • Choose a larger tool diameter
  • For solid carbide end mills and exchangeable-head mills, select a higher helix geometry (ap ≥ 45°)
  • Split axial cutting depth, ap, into more than one pass
  • Reduce feed, fz
  • Reduce cutting speed, vc
  • HSM requires shallow passes
  • Improve clamping of tool and workpiece

Crater wear
Excessive wear results in a weakened edge. Cutting edge breakthrough on the trailing edge results in a poor surface finish.
  • Diffusion wear due to cutting temperatures on the rake face that are too high
  • Select an Al203 coated grade
  • Select a positive insert geometry
  • Reduce the speed to obtain a lower temperature, then reduce the feed​

Plastic deformation
Plastic deformation of the edge, depression or flank
impression leads to poor chip control, poor surface
finish and insert breakage.
  • Cutting temperature and pressure too high
  • Select a more wear-resistant (harder) grade
  • Reduce cutting speed, vc
  • Reduce feed, fz

The part of the cutting edge not in cut is damaged by chip hammering. Both the top side and the support for the insert can be damaged, leading to poor surface texture and excessive flank wear.
  • The chips are deflected against the cutting edge
  • Select a tougher grade
  • Select an insert with a stronger cutting edge
  • Increase cutting speed, vc
  • Select a positive geometry
  • Reduce feed at the beginning of cut
  • Improve stability

Small cutting edge fractures (frittering) result in
poor surface finish and excessive flank wear.
  • Grade too brittle
  • Insert geometry too weak
  • Built-up edge
  • Select a tougher grade
  • Select an insert with a stronger geometry
  • Increase cutting speed, vc, or select a positive geometry
  • Reduce feed at the beginning of cut​

Notch wear​
Notch wear results in a poor surface finish and the risk of edge breakage.
  • Work hardening materials
  • Skin and scale
  • Reduce cutting speed, vc
  • Select a tougher grade
  • Use a stronger geometry
  • Use a cutting angle closer to 45 degrees
  • Use round inserts for best result
  • Use variable ap technique to prolong the wear

​​Thermal cracks
Small cracks perpendicular to the cutting edge
result in frittering and a poor surface finish due to temperature variations.
  • Intermittent machining
  • Varying cutting fluid supply
  • Select a tougher grade with better resistance to thermal shocks
  • Cutting fluid should be applied copiously or not at all​​

Built-up edge (BUE)​
Built-up edge results in a poor surface finish and cutting edge frittering when the BUE is torn away.
  • Cutting zone temperature is too low
  • Very sticky material, such as low-carbon steel, stainless steels and aluminum
  • Increase cutting speed, vc
  • Change to a more suitable insert geometry

Built-up edge (BUE)​
Workpiece material is welded to the cutting edge.
  • Low cutting speed, vc
  • Low feed, fz
  • Negative cutting geometry
  • Poor surface finish
  • Increase cutting speed, vc
  • Increase feed, fz
  • Select a positive geometry
  • Use oil mist or cutting fluid
We use cookies to enhance the experience on our website. More about cookies.