Spanish 
French 
German 
Simplified Chinese G41- Cutter Compensation Left
The G41 command enables cutter compensation to the left side of the programmed tool path.
G41 is a modal command and belongs to Group 7.
When cutter compensation is active, the cutter is offset to the left-hand side of the original tool path by an amount calculated from the active compensation parameters.
Cutter Compensation Calculation
The cutter compensation offset is calculated using three parameters that work together to define the final offset distance.
The offset calculation is performed using the following formula:
Toolpath Offset = (Tool Diameter + Wear Diameter) ÷ 2 + P Value
The Tool Diameter represents the nominal diameter of the cutter, such as a 10 mm end mill, and is defined in the F4 Tool Table. If cutter compensation is already applied in CAM software, this value is typically left as 0.
The Wear Diameter represents the amount of tool wear or size variation and is also defined in the F4 Tool Table. A negative value is used for an undersized tool, while a positive value is used for an oversized tool.
The P value represents the radius used to offset the tool path and is typically used in hand-written G-code. This value is added to the calculated radius from the Tool Diameter and Wear Diameter.
For a more detailed explanation of managing tools, refer to the section Managing Tool Diameter and Wear Values at the end of this page.
Syntax & Parameters
When the G41 command is issued, MASSO uses the Tool Diameter and Wear Diameter values assigned to the currently active tool.
When a P value is specified, it is added to the Wear Diameter offset and is treated as a radius value. If no P value is specified, the offset calculation uses only the Tool Diameter and Wear Diameter from the F4 Tool Table.
The Tool Diameter must always be a positive value.
The Wear Diameter must be entered as a negative value for an undersized tool and a positive value for an oversized tool.
Example Programs
N10 T1 M06 N20 G41
N10 T1 M06 N20 G41 P5
In this example, a P value of 5 mm offsets the cutter by 5 mm from the original tool path. If Tool Diameter and Wear Diameter values are assigned to Tool 1 in the F4 Tool Table, they are included in the offset calculation.
N10 T1 M06 N20 G00 X-50 Y-25 Z25 N30 G01 Z-5 F250 N40 G41 N50 X-25 (lead in) N60 X100 N70 Y-100 N80 X25 N90 Y25 N100 G40 N110 X25 Y50 (Lead out) N120 G00 Z25
In this example, cutter compensation is enabled after the tool is positioned at cutting depth. A linear lead-in move is used before cutting begins. Cutter compensation is cancelled using G40, and a lead-out move is performed to a safe location before retracting the tool.
The final lead-out move is not displayed as a compensated move once cutter compensation has been turned off.
Compensated Toolpath shown in Purple
Troubleshooting
If the compensated tool path displays loops or self-intersections, this indicates that the calculated cutter size is too large for the programmed geometry. In this situation, a smaller cutter should be selected that is more appropriate for the job.
Cutter too large Cutter size correct
Cutter Compensation Rules
Cutter compensation paths are calculated and displayed when the G-code file is loaded.
Outside corners are automatically radiused.
Cutter compensation is valid in the G17 XY plane only.
Cutter compensation is valid only for X and Y axis moves.
Z, A, or B axis movements must not be included while cutter compensation is active, as this may cause unpredictable results.
The tool must be moved to the required cutting depth before enabling cutter compensation.
Non-cutting commands, such as coolant on or off, must not be included while cutter compensation is active.
A linear lead-in move to a safe location is required before enabling cutter compensation.
A linear lead-out move to a safe location is required after cancelling cutter compensation.
The lead-out move is not shown on screen as a compensated move.
Both lead-in and lead-out moves must use linear motion only.
The lead-in and lead-out distance must be greater than the cutter radius.
A single arc command must not be used to cut a complete circle.
Both X and Y coordinates must be specified on the first move after cancelling cutter compensation to avoid unpredictable motion.
The jump-to-line feature must not be used while cutter compensation is active. To resume cutting, the program must be rewound to a point before cutter compensation was enabled.
The easiest way to understand G41 is to imagine standing behind the cutter as it moves away from you. When G41 is active, the cutter moves to the left-hand side of the programmed tool path.
Managing Tool Diameter, Wear Diameter, and P Value
MASSO cutter compensation has been designed for maximum flexibility and compatibility with both CAM-generated and hand-written G-code.
The Tool Diameter and Wear Diameter values assigned to the current tool are automatically applied whenever G41 is enabled.
The final cutter offset is always calculated using the Tool Diameter, Wear Diameter, and any P value specified in the G-code.
P Value Usage
The P value specifies a cutter radius directly in G-code. For example, a 10 mm cutter would use a P value of 5 mm.
This method is commonly used in hand-written G-code where it is easier to program the nominal geometry and allow the controller to apply the cutter offset.
In this scenario, the Tool Diameter in the F4 Tool Table is typically set to 0, and the cutter radius is controlled entirely using the P value.
If a Wear Diameter is also defined, it is included in the final offset calculation.
Although uncommon, the P value can be used together with Tool Diameter values if required for a specific application.
Tool Diameter Usage
When cutter compensation is handled in CAM software, the Tool Diameter value in the F4 Tool Table is usually set to 0.
When cutter compensation is not included in the G-code, such as in hand-written programs, the Tool Diameter value can be used to apply the cutter offset.
The Tool Diameter can represent either the actual measured cutter diameter or the nominal cutter diameter, with final size adjustment handled using the Wear Diameter.
Wear Diameter Usage
The Wear Diameter is used to fine-tune the effective cutter size as the tool wears.
A negative Wear Diameter value indicates that the tool is undersized.
A positive Wear Diameter value indicates that the tool is oversized.
For example, a 10 mm cutter with a Wear Diameter of ?0.5 mm results in an effective tool diameter of 9.5 mm.
A 10 mm cutter with a Wear Diameter of +0.5 mm results in an effective tool diameter of 10.5 mm.
