Service Home Tap Breakage - Troubleshooting Guide
Last updated: 03/29/2023

Tap Breakage - Troubleshooting Guide

Introduction

This document explains some of the most common causes for tap breakage.

Program Troubleshooting

  • The RPM may be too high:
    • Set the RPM to a maximum of 3000, or 150 inches per minute feed, whichever comes first.
    • The DT-1 can tap at up to 5000 RPM.
  • If you are using a tension-compression holder:
    • Use 90% of the actual feed calculated for the thread to allow constant pressure on the tap as it enters and exits the hole.
    • Use 90% of the actual feed calculated for the thread if the machine does not have the Rigid Tap option.
  • Check the feedrate:
    • The speed and feedrate must be precise to maintain the correct synchronization between the tool and the Z-axis.
  • Keep the R-plane no shorter than 0.200” ( 5 mm) to give the machine some space to synchronize and accelerate.
  • If tapping small holes:
    • Put the machine to high gear (M42).
    • Tapping small holes in high gear speeds up the tapping process.
    • The high gear has less mass in the drive train to start and stop.

Tap Troubleshooting

  • Spiral flute taps:
    • Spiral flute taps are designed to pull chips out of the hole and away from the cutting area.
    • They work well when tapping a blind hole.
  • Spiral point taps:
    • Spiral point taps are designed to push chips forward and into the hole away from the cutting area.
    • They work well when tapping a through hole.
    • They do not work well in blind holes because the tapping chips can pack into the bottom of the hole and cause the tap to bottom.
  • Tap run out:
    • Make sure the run out is correct for the tap.
    • Some taps break if the TIR is more than 0.001" (.03 mm).
  • Make sure the tap is designed for use on CNC equipment:
    • Spiral flute taps work well and will eject chips from the working area.
    • Roll taps are stronger than cut taps and are recommended for small diameter tapping.
    • Hand taps are not designed for use on CNC machines.
  • Check the tap holding:
    • If the tap holder is a collet, make sure the tap does not slip.
    • If the tap holder is a collet, make sure the tap is not running out.
    • Taps must be held with a positive-drive device.
    • Make sure the collet is specifically designed to hold taps.

Material Troubleshooting

  • Hard Materials:
    • If the material is very hard, do not use coolant.
    • Clear the chips out of the holes and use a cutting fluid.
  • Soft Materials:
    • Soft, gummy materials require a consistent cooling mix.
    • They may also require special tapping compounds.
    • Check the coolant concentrations with a refractometer.
    • Always follow the manufacturer's mixing directions or use tapping solutions.

Hole Troubleshooting

  • Check the hole depth:
    • Blind holes need be drilled at least 0.050” deeper than the tap is programmed to go.
    • The hole will be shallower than what is programmed because of the tip angle on the drill.
    • Setting an offset for the tip of the tool will make the hole shallow by the amount lost by the tip angle.
    • The program can compensate for this by drilling slightly deeper. This gives you the diameter required to the depth required.
  • Spot drill, then tap:
    • Spot drill a pilot hole before tapping.
    • This will insure that the drill is located accurately.
    • Drill the pilot hole slightly greater than the major diameter of the tap size.
  • Make sure the tap drill is the correct size:
    • For 75% of effective thread use this formula:
      • D - 1/N
      • D = major diameter of the tap
      • N = number of threads per inch
  • Hole dimensions:
    • A tapped hole with 75% of thread depth has only 5% less strength than 100% thread and takes only 1/3 of the cutting force of a 100% thread.
    • One and one half times the major diameter is the usual depth requirement for a tapped hole.
    • The strength of a threaded connection does not increase if the contact length is more than 1.5 times the diameter of the fastener.
    • Chances of breaking the tap increase dramatically when tapping more than one-and-a-half times the major diameter 

Machine Troubleshooting

  • Z Axis Overshoot and Drift:
    • Use an indicator and a simple, repeating incremental tapping program to test drift.
    • If the Z-Axis overshoots/drifts farther than what is programmed in the G84:
    • Parameter 120, SPINDLE ACC/DECEL adjusts the amount the Z axis can overshoot.
    • Parameter 144, RIG TAP FINISH DIST also adjusts the amount the Z axis can overshoot.
  • Rigid Tapping:
    • If the customer has rigid tapping, make sure Parameter 57:4 RIGID TAP is ON.
  • Peck Tapping:
    • If the customer is tapping the same hole more than once (peck tap), make sure Setting 133 REPEAT RIGID TAP is ON.
    • Prior to mill version 12.09 REPEAT RIGID TAP was turned on with Parameter 57:6.
  • Tap Retract:
    • Setting 130, TAP RETRACT SPEED, controls the speed at which the tap retracts.
    • Reduce the value in this setting if cross-threading or tearing occurs.
  • Spindle Encoder:

Coolant Troubleshooting

  • Tapping Compound:
    • If coolant may be the cause of the problem, program a series of holes and brush a tapping compound or tapping oil on the tap instead of coolant.
    • Tap Magic makes several different types of high quality tapping fluid.
  • Coolant Condition:
    • Always follow the coolant manufacturer's recommendations for mixing coolant.
    • Check the coolant concentrations with a refractometer.
    • Make sure the water has a low mineral content. Minerals in the water break down the quality of the coolant and reduce the coolant's effectiveness.