Tool Nose Radius and Wear Offset

Classic Control - Lathe Operator's Manual

The Online Interactive Operator's Manual is currently available in English only.

A PDF version of the Operator's Manual is available for download in multiple languages. Click the link below to view the Operator's Manual in your language. Click "Continue" to view the online version in English.

Get a translated PDF Download Continue

Each turning tool that uses tool nose compensation requires a Tool Nose Radius. The tool tip (tool nose radius) specifies how much the control is to compensate for a given tool. If standard inserts are being used for the tool, then the tool nose radius is simply the tool tip radius of the insert.

Associated with each tool on the geometry offsets page is a Tool Nose Radius Offset. The column labeled Radius contains the value for the tool nose radius of each tool. If the value of any tool nose radius offset is set to zero, no compensation is generated for that tool.

Associated with each radius offset is a Radius Wear Offset, located on the Wear Offset page. The control adds the wear offset to the radius offset to obtain an effective radius that is used for generating compensated values.

Small adjustments (positive values) to the radius offset during production runs should be placed in the wear offset page. This allows the operator to easily track the wear for a given tool. As a tool is used, the insert generally wears so that there is a larger radius at the end of the tool. When replacing a worn tool with a new one, clear the wear offset to zero.

It is important to remember that tool nose compensation values are in terms of radius rather than diameter. This is important when tool nose compensation is canceled. If the incremental distance of a compensated departure move is not twice the radius of the cutting tool, overcutting occurs. Always remember that programmed paths are in terms of diameter and allow for twice the tool radius on departure moves. The Q block of canned cycles that require a PQ sequence is often a departure move. The following example illustrates how incorrect programming results in overcutting.


  • Setting 33 is FANUC

Tool Geometry X Z Radius Tip
8 -8.0000 -8.00000 .0160 2


% o30411 (TOOL NOSE RADIUS AND WEAR OFFSET) ; (G54 X0 is at the center of rotation) ; (Z0 is on the face of the part) ; (T1 is a boring bar) ; (BEGIN PREPARATION BLOCKS) ; T101 (Select tool and offset 1) ; G00 G18 G20 G40 G80 G99 (Safe startup) ; G50 S1000 (Limit spindle to 1000 RPM) ; G97 S500 M03 (CSS off, Spindle on CW) ; G00 G54 X0.49 Z0.05 (Rapid to 1st position) ; M08 (Coolant on) ; (BEGIN CUTTING BLOCKS) ; G96 S750 (CSS on) ; G41 G01 X.5156 F.004 (TNC left on) ; Z-.05 (Linear feed) ; X.3438 Z-.25 (Linear feed) ; Z-.5 (Linear feed) ; X.33 (Linear feed) ; G40 G00 X0.25 (TNC off, exit line) ; (BEGIN COMPLETION BLOCKS) ; G00 Z0.1 M09 (Rapid retract, coolant off) ; G53 X0 (X home) ; G53 Z0 M05 (Z home, spindle off) ; M30 (End program) ; %

TNC Departure Cutting Error

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.