If your tool has excessive wear, the cutting forces generated by the cut will increase. These increased cutting forces can lead to chatter during the cut. 

Inspect your tool and replace it if necessary. 

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 to alert the operator to replace the tool before it negatively affects your machining process.

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

When the cutting speed (surface feet per min or meters per min) is too high or the feedrate (feed per revolution) is too low, the cut can become unstable and begin to resonate, leaving a chattered surface finish.

Reduce the cutting speed or increase the feed rate to stabilize the cut. Refer to the tooling manufacturer's instructions for guidance as to the best speeds and feeds to use for the tooling and workpiece material. Test-run your application and use spindle speed and feed overrides to find a speed/feed combination that does not chatter.

 Note: Check the tool insert box for cut parameter recommendations. Many manufacturers print the cut information directly on the insert box label.

 Note: If you are still experiencing high runout and poor surface finish problems after troubleshooting, see the Spindle - Lathe Troubleshooting Guide.

Insert selection is critical for a stable cut. The chip-breakers, coatings, radius sizes, geometry, and carbide grade must be designed for the workpiece material. Improper inserts can cause problems with surface finish, tool life, and chatter

Corrective Action:

Consult with your cutting tool vendor to select the proper insert geometry, radius size, coating and carbide grade for you application.

If the workpiece is not properly supported, it will begin to vibrate and introduce chatter into the cut. 

As a general rule, if the portion of the workpiece that extends past the chuck exceeds a diameter-to-length ratio of 3:1, use a tailstock to stabilize the cut. 

If the length-to-diameter ratio of your workpiece exceeds 10:1, you may need to use the additional support of a steady rest, different workholding, or a different machining strategy to stabilize the cut.

Helpful Hint:
Consider using the Spindle Speed Variation (SSV) feature to disrupt chatter.

For more details on tailstocks watch Tailstock Fundamentals: How to use the Tailstock on a Haas Lathe.

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.

Use the optional A and P codes with a G76 threading cycle to control the infeed angle (A) and cutting method (P). 

The A value specifies the infeed angle, or the tool nose angle, for the thread. This value can range from 0 to 120 degrees; do not use a decimal point. If you do not specify an A value, the control assumes zero.

The P value specifies the cutting method. The options are P1, P2, P3 and P4. These control whether the depth of cut is a constant depth with each pass, or a constant cutting amount that reduces the depth of cut the deeper into the thread it goes. The P value also specifies single edge or double edge cutting. If you do not specify a P code, the control selects the P code designated in Setting 232.

• P1 Single edge cutting, cutting amount constant
• P2 Double edge cutting, cutting amount constant
• P3 Single edge cutting, cutting depth constant
• P4 Double edge cutting, cutting depth constant 

Helpful Hint:

To reduce chatter while threading, use an A value 1-3 degrees less than the included angle of the thread; for example, use an A57, A58 or A59 to cut a 60-degree included angle thread. This allows for clearance on the back side of the insert so it does not contact the thread form until the final depth cut. 

Refer to G76 Threading Cycle, Multiple Pass (Group 00) - Lathe for more details on threading.

The insert geometry, insert grade and/or insert shim are incorrect for the application.

Corrective Action:

Consult with your tooling manufacturer for recommendations on proper tool selection for your application, and make adjustments where necessary.

Helpful Hint 1:

Threading inserts come in many different shapes and sizes. Topping inserts are the most common threading inserts used on a CNC machine. Topping inserts cut one full thread form at a time, and they are designed for a specific pitch.

Be sure to use the correct insert for your application.

Helpful Hint 2:

Check under the insert for a seat, sometimes referred to as a shim. This seat is ground to an angle. Different thread diameters require different seat angles. Check with the insert manufacturer to be sure that you are using the correct seat for the thread being cut.

Setting 99 (THREAD MIN CUT) and setting 86 (THREAD FINISH ALLOWANCE) control the minimum roughing depth-of-cut and the final finish pass depth-of-cut for a G76 threading cycle.

Corrective action:

Use an infeed chart from the tooling manufacturer to set the values for Setting 86 and 99.

This chart specifies the minimum and final cut values for a specific thread size, as well as the total number of depth cuts for roughing.

The OD or ID threading tool is too long, or it is not properly supported.

Corrective Action:

Adjust the OD stick tool holder so that the tool holder’s projection length from the turret is as short as possible. If you must use a longer stick tool for clearance, consider using a Haas Twin Turn or Extended Twin Turn BOT holder to fully support the stick tool. You can get these holders on parts.haascnc.com.

Adjust the ID boring bar holder so that the tool’s projection length from the tool older is as short as possible. The material type of the bar will affect its stability. A steel boring bar is stable up to a stick-out of 3 times the diameter. A carbide boring bar is stable at a length up to 5 times its diameter. If you must exceed these limits, you must compromise your cut parameters to compensate for the reduced stability—reduce the depth-of-cut, or spindle speed to compensate.

Helpful Hints:

If you need to use a bushing for the boring bar, use a split bushing to increase bar support.

Special vibration-dampening boring bars are available when you need an extreme length-to-diameter ratio to machine an ID thread.

A linear guide, the ball screw, or the ball nut is damaged:

Before removing the waycovers, make sure these items on the machine are within specification. If they are not, make adjustments and test the machine.

1. Machine Level
2. Alignment of the Spindle
3. Alignment of the Turret
4. Alignment of the Tailstock

If the problem continues, remove the way covers and examine the linear guides, the ball screw, and the ball nut for damage, movement, or signs of a crash.

 Note: Damaged or loose bearings in the trucks for the linear guides can cause the machine to chatter during aggressive cutting. The linear guide pads on the machine should not have any side to side / up and down movement over 0.002".

If the linear guides, the ball screw, or the ball nut are damaged or loose, replace them.

The quill has play inside the tailstock body. (ST-20/30):

If the quill has play, replace the complete quill assembly. The assembly is not field serviceable.

Refer to: Lathe - Hydraulic Tailstock - Troubleshooting Guide