2.4 Cutter Radius Compensation (G41/G42/G40) & Tool Length Offsets (G43/G49)

Key Takeaways

  • G43 H selects a tool-length value and adds it to the commanded axis position. Use the H register intended for the loaded tool and verify Haas Setting 15.

  • Haas NGC from version 100.21.000.1100 normally applies the tool offset and updates it at a tool change. G49 or H00 explicitly cancels mill length compensation.

  • With positive effective D, G41 moves the tool left of the programmed path in G17 and G42 moves it right. A negative effective D reverses these sides.

  • On a Haas mill, Setting 40 determines radius or diameter entry. The effective offset combines geometry and wear, with half the entry applied in diameter mode.

  • Plan G01 XY entry and cancellation moves long enough for the compensation and clear of material during each transition. Check material side and spindle rotation to determine climb or conventional milling.

Last updated: November 2026

2.4 Tool Length and Cutter Radius Compensation

A program expresses where the cut belongs on the workpiece. The control must translate that request into a position for the tool assembly. Tool-length compensation accounts for the distance from the chosen measuring reference to the tool tip. Cutter radius compensation moves the tool center away from a programmed contour. The examples use a three-axis Haas mill.

Tool Length: G43, H and G49

G43 H03 selects the length offset in register H03 and adds the effective value to the commanded axis position. G44 subtracts its selected value. G49 or H00 cancels mill length compensation as documented by Haas. Applying or canceling compensation changes how commanded coordinates map to the tool. Verify the active state and include any intentional change in the clearance plan.

For example, assume G54 Z0 has a machine coordinate of −15.250 in in a system using full spindle gauge-line measurements. Tool 3 has an effective length of +4.000 in below the gauge line. To put the tip at work Z+1.000 in, the gauge line must be at −15.250 + 1.000 + 4.000 = −10.250 in. If a 3.500-in effective length were applied to that actual tool, the gauge line would instead reach −10.750 in. The tip would be 0.500 in lower than the intended target. These examples assume ordinary positive Z away from the part, no other shifts, and the measured offset convention in Work Coordinates and Fixture Offset Setting.

In current Haas NGC software beginning with 100.21.000.1100, the mill normally applies a length offset and updates it to match the newly loaded tool on a tool change, unless explicitly canceled. The active offset and group state persist through power cycles. An explicit H selection can request a different stored length. If Setting 15 (H and T Code Agreement) is on, an H/T mismatch triggers an alarm. With it off, a wrong H can give the wrong tool-tip position. Verify the actual control revision and selected H even when tool change is automatic.

Cutter Side: G41, G42 and D

For Haas 2D cutter compensation in G17, look in the direction of tool travel. With a positive effective offset, G41 puts the tool center to the left of the programmed path and G42 puts it to the right. A negative effective offset switches sides. G40 cancels compensation. With it canceled, the XY path specifies the tool center. When working from a CAM program, determine whether the numbers already describe a tool-center path and whether the D register is meant to contain the full tool size or just a small correction.

The D address selects a register. Haas sums its geometry and wear values. In diameter mode, selected by Setting 40, an effective entry of +10.000 mm produces a 5.000 mm shift. In radius mode, +5.000 mm produces the same shift. Settings such as Setting 58 also affect how controls handle short moves and corners.

Determine the Cut from its Geometry

Suppose the programmed path travels east along Y0 and the remaining part is south of the edge. The cutter center belongs north of the edge: left of eastward travel, so use G41 with a positive full-radius offset. With default forward clockwise rotation viewed from +Z, the cutting edge at the south side of the cutter travels west at the contact. Seen from the tool, the material also feeds west. That same-direction contact is climb milling. It normally produces a thick-to-thin chip in single-sided peripheral engagement. Reversing spindle rotation changes the engagement even if the offset selects the same side. A slot can engage both sides. Determine climb or conventional milling from actual tool rotation, feed, and material contact.

Enter and Leave Compensation

On the Haas mill, enable or cancel 2D compensation on a G01 XY move. Plan a straight motion at least as long as the compensated amount and verify that the swept cutter clears the stock and fixture during the transition. Avoid arcs for activation or cancellation. An inside arc smaller than the compensated radius can cause an interference alarm. Check the programmed corner, the actual cutter and the specified compensation.

Worked Straight-Edge Trace

In this Haas G17 graphics example, the nominal boundary runs from X0.0 to X40.0 at Y0.0, and the part lies to its south. At the starting clearance the tool center is at X−20.0, Y0.0. There are no stock or fixtures in either transition area. D03 holds +10.0 mm effective diameter. The path below stays at a verified Z.

G21 G17 G90 G94 G40
G01 G41 D03 X-10.0 Y0.0 F400.0
G01 X50.0 Y0.0
G01 G40 X65.0 Y0.0

The 10-mm activation move exceeds the 5-mm compensated shift. Across the wall the tool center is at Y+5.0, so its south cutting edge lies at Y0.0 with a 10-mm cutter. By X50.0 the cutter has moved beyond the part. The 15-mm departure returns the center to the uncompensated Y0.0 in clear space. Check both ends of the wall and the full transition envelope before applying this pattern to a cutting move.

Sources: Haas mill cutter compensation, Haas G43/G44 and NGC behavior, Haas H/T agreement, and Sandvik Coromant milling engagement.

Loading diagram...
G41 Lead-In and G40 Lead-Out Vector Sequence
Test Your Knowledge

On a Haas mill, a G17 contour travels in +X with effective D positive. If the cutter belongs on the +Y side, which code selects it?

A

G40

B

G41

C

G42

D

G43

Test Your Knowledge

What does H03 select in G43 H03 Z1.000 on a Haas mill?

A

The tool-length offset in register 3

B

An arc radius of 3 inches

C

The fixture offset G56

D

The third coolant nozzle position

Test Your Knowledge

Which activation move meets the basic Haas 2D compensation rule when the effective shift is 5 mm and the entry area is clear?

A

A 5-mm radius G02 arc

B

A straight 2-mm G01 XY entry

C

A straight 8-mm G01 XY entry

D

A rapid Z-only entry

Test Your Knowledge

Tool 4 is in a Haas mill, Setting 15 is on, and a block explicitly calls G43 H01. What happens?

A

The control applies H01 regardless of the tool.

B

The program always substitutes H04 silently.

C

The control signals an H/T mismatch alarm.

D

The control applies a diameter wear offset from D01.

Sections you finish are checked off in the contents.