Knife Problems and Countermeasures in CNC Processing

• 1
  Quick reference: symptom, cause, and countermeasure
• 2
  Flank wear and rake wear: the slow failure
• 3
  Chipping and micro-breakage at the cutting edge
• 4
  Built-up edge, especially on aluminium and soft steels
• 5
  Deflection, chatter, and dimensional drift
• 6
  Breakage, tool pull-out, and the post-mortem
• 7
  A 6-step countermeasure routine for the shop floor

Flank wear is the normal end of a tool's life. The wear land grows on the relief face, rubbing against the finished surface. If you inspect a tool under a loupe every 30 minutes of cut time, you can watch it happen. On 6061 aluminium at 900 m/min and 0.15 mm/tooth, a carbide end mill might last 4 to 6 hours before the wear land reaches 0.2 mm. On 17-4PH stainless at 60 m/min, that drops to 40 to 60 minutes.

The symptom is easy to miss at first. Surface finish starts drifting from Ra 0.8–1.6 μm toward Ra 3.2 μm. The spindle load creeps up 5 to 8 percent. By the time you hear a change in pitch, the wear land is already past 0.3 mm and the tool is rubbing, not cutting. Heat goes into the part instead of the chip, and dimensions start to walk.

The countermeasure is boring but effective. Set a cut-minute limit per edge and index on schedule, not on sound. For stainless and titanium, that limit is usually 30 to 45 minutes per edge. For aluminium, 4 to 6 hours. Log it. A tool that broke on the last pass of a 6-hour cycle almost always ran past its limit.

Rake face wear is different. It forms a crater behind the cutting edge, and the edge gets weak before the flank is anywhere near its limit. This shows up on steels and cast irons at high speed. If you see a crater deeper than 0.1 mm, the speed is too high for the coating. Drop 15 to 20 percent and check again.

Chipping is a sudden event, not a gradual one. A small piece of the edge breaks away, usually at the corner radius or at the point where the tool enters the cut. You will see it as a bright spot on the edge under a loupe, or as a sudden change in surface finish on one section of the part.

The most common cause is entry shock. When a tool plunges straight into a solid corner, the edge takes the full impact at zero chip thickness. That is the worst possible condition for carbide. The fix is arc entry or ramp entry, and a feed rate at the corner that is 50 to 70 percent of the straight-line feed. Most CAM systems call this feed reduction, and most programmers leave it at 100 percent by default.

The second cause is runout. If the tool has more than 0.02 mm of runout at the tip, one flute does most of the cutting and chips first. Check runout with a dial indicator on the flute, not on the shank. If it is over 0.02 mm, clean the holder taper, reseat the collet, and check again.

The third cause is the material itself. Hard spots, inclusions, and cast skin will chip an edge that is otherwise fine. On castings and forgings, take a 0.5 mm skin cut at reduced feed before the main pass. It costs 20 seconds and saves the tool.

Built-up edge (BUE) is welded material stuck to the cutting edge. It grows, breaks off, and takes a piece of the coating with it. On aluminium, it looks like a rough, smeared surface with a dull, matte finish. On low-carbon steel, it shows up as a rough patch that appears and disappears as the edge loads and unloads.

The cause is a combination of low cutting speed, high feed per tooth, and coolant that does not lubricate. Aluminium alloys like 6061 and 5052 are prone to this, especially with uncoated carbide. The pressure and temperature at the edge are enough to weld the chip to the tool, and the weld is stronger than the tool surface.

The countermeasure is to raise the surface speed and use a coating that resists aluminium adhesion. PVD coatings like TiAlN or diamond-like carbon work well. On a 12 mm end mill in 6061, going from 300 m/min to 900 m/min usually eliminates BUE completely. Use a high-pressure coolant stream aimed at the cutting edge, not at the chip.

If the part has thin walls or deep pockets where you cannot raise speed, switch to a polished, uncoated tool with a high rake angle. These geometries cut aluminium cleanly at lower speeds and are less likely to weld. They wear faster, but the surface finish is worth it.

Deflection is not a tool failure in the sense of a broken edge, but it causes the same result: a part that does not meet tolerance. The tool bends under cutting force, and the finished wall is tapered or undersized. On a deep pocket with a long tool, the deflection at the tip can be 0.05 mm or more, which is 10 times our ±0.005 mm tolerance.

Chatter is deflection that oscillates. You hear it as a squeal or a growl, and you see it as regular marks on the wall. The marks are spaced at the natural frequency of the tool-holder-spindle system. The fix is to change the frequency or reduce the force. Shorten the overhang, increase the tool diameter, or reduce the radial depth of cut.

A common mistake is to slow the spindle down when chatter starts. That often makes it worse because it moves the tooth-passing frequency closer to the natural frequency. The better move is to increase the speed by 10 to 20 percent and reduce the feed, or to change the radial engagement from 50 percent to 30 percent of the tool diameter.

For deep pockets, use a roughing strategy that leaves 0.3 to 0.5 mm of material on the wall and floor. Then take a finishing pass with a short, rigid tool. The finishing pass removes the deflection marks and holds the tolerance. We do this on every deep pocket that goes past 3 times the tool diameter.

Breakage is the most expensive failure because it usually takes the part with it. A broken tool in a deep pocket means scrapping the part or spending hours with a spark eroder. The cause is almost always a combination of factors: too much overhang, too much feed, and a material condition that was not planned for.

Tool pull-out is a specific type of breakage. The tool slides out of the collet under high axial load, usually during a deep drilling cycle or a heavy face mill cut. The symptom is a sudden change in Z position and a loud noise. The countermeasure is to use a holder with a positive stop, like a Weldon or a hydraulic holder, and to check the collet nut torque before every long cycle.

After any breakage, do a short post-mortem. Check the fracture surface: a dull, grey surface means fatigue, and a bright, crystalline surface means overload. Check the chip shape: long, stringy chips mean the feed is too low, and thick, blue chips mean the speed is too high. Check the coolant: if the tool is discoloured, the coolant was not reaching the edge.

We log every breakage with the tool number, the material, the cut parameters, and the time in cut. After 50 or so entries, patterns show up. On one aluminium job, we found that 80 percent of breakages happened on the first part after a tool change. The cause was that the new tool was longer than the old one, and the operator did not reset the tool length offset.