G41 and G42 Tool Nose Radius Compensation

G41 Example Program

The tool nose radius and the amount of offset is entered into the Secondary Offsets Table. Press F9 in Auto Mode to access the table.

An excerpt from the Secondary Offesets Table is illustrated below, along with an example program and toolpath.

In the Secondary Tool Offset Table:

• The "X" value is the diameter value (twice the TNR) to offset the tool in the X-axis
• The "Z" value is the amount to offset the tool in the Z-axis
• The "R" value is the tool nose radius

In the program:

• The "D" value is the secondary offset tool that is called

G41 and G42 Offsets Explained

Left or right compensation is determined by viewing the toolpath from the cutter's point of view. The tool is moved away from the part to accommodate the tool nose radius (see illustration below):

• If the tool is moved away from the part to the LEFT, G41 is used.
• If the toolis moved away from the part to the RIGHT, G42 is used.

A simple OD part is illustrated below, using the same cutter on both sides of part, cutting both toward and away from the spindle.

The canned cycle (g41 or g42) creates a toolpath that follows the contour of the part, offset by the "R" value set in the Secondary Offset Table.

To put the centerline of the tool nose radius on that toolpath, the program applies the "X" and "Z" values:

• If the tools is working the frontside of the part, the "X" will be minus.
• If the tool is working the backside of the part, the "X" value will be plus.
• If the tool is working a face away from the spindle (plus-z) the "Z" value will be minus.
• If the tool is working a face toward the spindle (minus-z) the "Z" value will be plus.

The sign (plus or minus) of the "X" and "Z" values is to move the tool toward the part the amount of the TNR.