Mill Tool Life Troubleshooting - Drill

The Tool is Dull

It is normal for tools to wear over time. In a stable machining process the tool wear is predictable. This will allow you to use the Tool Life Management systems that come standard in your Haas control. The tool life information can be input in to the Haas control so that your operator will be alerted to replace the tool before the dull tool negativity effects your machining process. 

Refer to the Tool Life Management section for details on how to use these systems. 

The RPM & Feedrate are Not Optimal

If the RPM and feedrate are not set correctly excessive heat will be produced, this heat will damage the tool and cause premature wear, furthermore it may lead to chatter or surface finish issues.  

Make sure that your feedrate and RPM are correct for the tooling and the workpiece material. Refer to your tooling manufacturer's documentation for the best cut parameters to use.

A cutting speed (Vc) that is too high has the most detrimental effect on your tool life. 

Cutting Speed Too High

  • Rapid flank wear
  • Poor finish
  • Rapid crater wear
  • Plastic deformation

Cutting Speed Too Low

  • Built-up edge
  • Dulling of edge
  • Uneconomical
  • Poor surface finish


The feed rate (fn) has a moderate effect on the tools life.

Feed Rate Too Light

  • Stringing chips
  • Rapid flank wear
  • Built-up edge
  • Uneconomical

Feed Rate Too Heavy

  • Loss of chip control
  • Poor surface finish
  • Crater wear
  • Plastic deformation
  • High power consumption
  • Chip welding
  • Chip hammering

Incorrect Peck Depth - Mill

A peck depth (ap) that is either too shallow or too deep leads to shorter tool life.
A peck that is too shallow wears the drill prematurely. This is because the majority of the wear on a drill happens during the initial chip creation when the drill enters the workpiece material. As far as the tool life is concerned, every peck is like drilling a new hole. 

If the peck is too deep, the drill may not be able to properly clear the chips. This leads to chip packing, which can prevent coolant from reaching the tool tip. This can also cause the drill to break, because the chips have nowhere to go.

As a general rule with carbide drills, the first peck should be 3 times the diameter of the drill (3 x d) and the subsequent pecks should be 1 times the diameter (1 x d).  Your pecking depth requirements will vary depending on your workpeice material and drill geometry. Consult with your tooling manufacturer to determine the appropriate pecking requirements for your application.    

For deep holes, use IJK to define the pecks instead of Q.

When you specify I, J, and K, the first peck cuts in by the amount of I. The depth of each subsequent peck in the cycle gets reduced by amount J, down to the minimum cutting depth K. Do not use a Q value when you use I, J, and K.

Note: Coolant-fed drills typically do not require pecking to clear the chips. 

The Drilling R Plane is Too Close to the Workpiece - Mill

The positioning moves between hole locations in a canned cycle are rapid movements. If the R plane is too close to the workpiece, the tool can begin to feed down before the axes reach the correct hole location. This can cause the tool to hit the edge of the hole as it enters, or it could start drilling/tapping at the wrong location.

Corrective Action:

Increase the R plane to a minimum of .100" (2.54mm) above the surface so that the axes are in position before the canned motion starts.

Coolant Issues

Incorrectly aimed coolant nozzles or obstructions in the stream can prevent coolant from reaching the cutting area. Adjust your coolant nozzles to deliver coolant to the cutting area.

Be sure to use the recommended coolant mixture concentration in your applications. If your concentration is too lean, the reduced lubricity can negatively affect your tool life and surface finish.
There are many different coolants for different applications and materials. Contact your coolant dealer for advice.

Refer to the Machine Tool Coolant Series page for videos and articles about maintaining your coolant system.

Excessive Drill Runout - Mill

Excessive runout on a tool will cause an inconstant load on the tool as it rotates. This can lead to premature tool wear, accuracy, and surface finish issues. 

Tool runout should not exceed 0.0003" (0.076 mm). The tool runout can be checked by placing a dial indicator on the tool and rotating the spindle by hand.   

Be aware: Many service and repair procedures should be done only by authorized personnel. The service technicians at your Haas Factory Outlet (HFO) have the training, experience, and are certified to do these tasks safely and correctly. You should not do machine repair or service procedures unless you are qualified and knowledgeable about the processes.

Danger: Some service procedures can be dangerous or life-threatening. DO NOT attempt a procedure that you do not completely understand. Contact your Haas Factory Outlet (HFO) and schedule a service technician visit if you have any doubts about doing a procedure.