What are I and J in G-code arcs?

I and J are the incremental offsets from the arc start point to the arc center along the X and Y axes. Most controllers use incremental I and J by default in the XY plane, so I equals center X minus start X and J equals center Y minus start Y. This tool outputs them in that incremental form.

Why are there two possible arcs?

A start point, end point, and radius do not define a unique arc, because the center can sit on either side of the chord connecting the points. That gives two centers and two arcs, one shorter and one longer. The tool shows both and marks the shorter solution.

What is the difference between G02 and G03?

G02 cuts a clockwise arc and G03 cuts a counter-clockwise arc, both viewed looking down the Z axis in the XY plane. The tool reports the correct direction for the minor arc to each center; to take the major arc the long way around, you reverse the G02 or G03 code.

Why does it say my radius is too small?

An arc must reach both endpoints, so its radius cannot be smaller than half the straight-line distance between them. If you see that warning, increase the radius to at least the half-chord value the tool reports, or move the endpoints closer together.

Does this work for the YZ or XZ plane?

This calculator targets the default XY plane used with G17, which covers the large majority of arc programming. For YZ work with G19 or XZ work with G18 the same geometry applies but the offset letters change to J and K or I and K respectively.

What is the G-Code Arc (I/J/K) Calculator?

Takes an arc start point, end point, and radius and computes the incremental I and J center offsets needed for G02 and G03 CNC arc moves in the XY plane. Shows both possible arc solutions with sweep angle, marks the shorter one, and outputs a ready-to-paste G-code line. Runs in your browser. It runs free in your browser on Gera Tools, with nothing uploaded.

G-Code Arc (I/J/K) Calculator

Name: G-Code Arc (I/J/K) Calculator
Creator: Gera Tools
License: https://creativecommons.org/licenses/by/4.0/

Get one useful tool a week

Like this tool? Enter your email and we'll send you one genuinely useful Gera tool a week — plus a link to come back to this one. No spam, one-click unsubscribe any time.

CNC controllers cut arcs with circular interpolation, and the trickiest part of hand-coding one is computing the I and J center offsets. This tool takes a start point, an end point, and a radius, computes the exact I and J values for both possible arc solutions, and outputs a ready-to-paste G02 or G03 line.

How it works — the geometry

The arc center must be equidistant from both endpoints, so it lies on the perpendicular bisector of the chord connecting them. Using the chord length and the radius, the distance from the chord midpoint to the center is found by Pythagoras, giving two centers — one on each side of the chord:

chord  = distance(start, end)
half   = chord / 2
a      = sqrt(radius² − half²)
center = midpoint ± a × (unit perpendicular to chord)
I      = center X − start X
J      = center Y − start Y

For each center the tool measures the swept angle in both directions to decide whether the minor arc is clockwise (G02) or counter-clockwise (G03), and marks the solution with the smaller sweep angle as the shorter arc.

Worked example

For a start point at (0, 0), end point at (10, 10), and radius 10:

Chord length = sqrt(10² + 10²) ≈ 14.14
Half-chord = 7.07; distance from midpoint to center = sqrt(10² − 7.07²) ≈ 7.07
Two centers: (10, 0) and (0, 10)

This gives two 90° arcs going in opposite directions:

Solution	Center	I	J	Code	Sweep
Minor arc 1	(10, 0)	+10.0	0.0	G02	90°
Minor arc 2	(0, 10)	0.0	+10.0	G03	90°

Both are 90° sweeps here (equal for a symmetric case). Choose the one whose bulge direction matches your intended toolpath, then copy the G-code line:

G02 X10.0 Y10.0 I10.0 J0.0 F200

Controller compatibility and edge cases

Incremental vs absolute I/J. The output uses incremental I and J (offset from the arc start to the center), which is the default on Fanuc, Haas, Mazak, LinuxCNC, and most other common controllers. If your machine uses absolute arc center mode (enabled by G90.1 on some Fanuc systems), use the printed center X/Y coordinates as I/J instead.

Radius too small error. An arc’s radius cannot be smaller than half the chord between the endpoints — the geometry has no solution. If you see this warning, either increase the radius or move the endpoints closer together.

Full circles. When start and end are the same point, I and J can define a full-circle arc. Most controllers require a full-circle move to be programmed as a single 360° arc with no endpoint specified, which this tool does not generate — use your CAM software for full circles.

G18 and G19 planes. This calculator targets the G17 XY plane, the default for most milling operations. For G18 (XZ plane) or G19 (YZ plane), the same geometry applies but the offset letters swap: I/K for G18 and J/K for G19. Verify your active plane modal before using the output.