We use technical and security cookies and, only if you accept, analytics with no cross-site tracking. More in the Cookie policy and Privacy policy.
We use first-party cookies and technical storage to make the site work, Google reCAPTCHA security technology and, only if you accept, Vercel analytics (no cookies, no cross-site tracking). You can accept or reject analytics; both options are equivalent and you can change your choice at any time. More info: Cookie policy, Privacy policy, Legal notice and Terms and conditions.
G02 cuts a circular arc clockwise, from wherever the tool is to the end point you program, in the active plane and at feedrate F. You give the control the center of the arc in one of two ways: with I, J and K, which are the distance from the start point to the center measured axis by axis, or with R, which is the radius. And clockwise is always judged looking from the positive side of the axis perpendicular to the plane: in G17, from +Z looking down.
For reference only: syntax changes with the control, the post-processor and the machine parameters. Check the official manual and run a simulation before cutting. Legal notice.
In G17 (XY), judge direction looking from +Z toward the plane. I and J locate the center relative to the start point; R specifies the radius.
Check the arc direction and compare G02 with G03 in the G-code simulator and editor.
Fanuc (milling)
G02 X20. Y60. I20. J0. F350I and J are incremental from the start point toward the center, even when the program is in G90. Only G90.1 changes that and makes them absolute: a mode best left alone, because an arc written for one does not work in the other.
Haas (milling)
G02 X20. Y60. R20. F350Same syntax as Fanuc. With R, the control picks the arc smaller than 180 degrees if R is positive and the larger one if it is negative. R is no good for a full circle: there you have to use I and J.
Fanuc / Haas (turning)
G02 X40. Z-5. R2. F0.15On a lathe you work in the G18 plane, so the pair of center letters is I (in X) and K (in Z). Watch out for I: it is measured in radius even though the program X values are in diameter. For small corner radii almost everyone uses R.
Siemens 840D / 828D
G2 X20 Y60 CR=20 F350Siemens uses G2 and writes the radius as CR=. It also takes I/J for the center, AR= to give the opening angle, and polar programming. A negative CR selects the arc larger than 180 degrees, just like a negative R on Fanuc.
Heidenhain TNC (Klartext)
CC X+20 Y+40 / C X+20 Y+60 DR-In Klartext you declare the center first with CC and then the arc with C and the direction: DR- clockwise and DR+ counterclockwise. CR lets you give the radius directly, and RND rounds the corner between two straight lines without working any point out.
| Letter | What it sets | Unit |
|---|---|---|
| X Y Z | End point of the arc, in absolute coordinates under G90. If you write the third axis on top of the two plane coordinates, the arc stops being flat and becomes a helix. | mm / in |
| I J K | Distance from the start point to the center of the arc, measured axis by axis: I in X, J in Y, K in Z. They are signed and only the two of the active plane are used (I and J in G17, I and K in G18, J and K in G19); the one that is zero can be left out. | mm / in, incremental from the start point |
| R | Radius of the arc, an alternative to I J K. Positive for the short arc (180 degrees or less) and negative for the long one. It is no good for a full circle. | mm / in |
| F | Feedrate along the arc. It is modal, just like in G01, so leave it out and it is inherited from the previous block. | mm/min under G94, mm/rev under G95 |
| G17 / G18 / G19 | Plane the arc is cut in. It decides which pair of I J K is used and from which axis the clockwise direction is judged. The wrong plane is the commonest cause of an arc alarm. | modal, no units |
Finish pass around the outside profile of an 80 x 60 mm aluminum plate with a 20 mm radius in the top left corner. A 12 mm cutter with offset D01 = 6.0 mm, compensation to the left active and the path running clockwise seen from above, which with M03 is climb milling. The same arc is shown written with I J and with R so you can see the two are equivalent.
O0102 (ESQUINA EN R20 CON G02) | ( Program header. ) |
G21 G17 G40 G49 G80 | ( Millimeters and XY plane. Declaring the plane before an arc is not a formality: the center letters and the direction of rotation both hang off it. ) |
G91 G28 Z0. | ( Z to the reference point before the change. ) |
T1 M06 | ( 12 mm cutter. ) |
G90 G54 G00 X-20. Y20. | ( Positioning clear of the part, on the extension of the left wall. ) |
G43 H01 Z50. M03 S3500 | ( T1 length offset and spindle on. ) |
G00 Z-4. M08 | ( Drops to the depth of cut while still clear of the material. ) |
G01 G41 D01 X0. Y20. F400 | ( Turns compensation on to the left in a 20 mm straight lead-in, well above the 6 mm cutter radius. ) |
G01 Y40. | ( Climbs the left wall X0 up to where the radius starts. The arc begins right here, at X0 Y40. ) |
G02 X20. Y60. I20. J0. F350 | ( The arc. I20 and J0 say the center sits 20 mm to the right and 0 in Y from the start point, that is at X20 Y40. It ends at X20 Y60 turning clockwise seen from +Z. ) |
(G02 X20. Y60. R20. F350) | ( The same arc written with a radius. Since it spans 90 degrees, less than 180, R is positive. Both forms give exactly the same path. ) |
G01 X80. | ( Top wall Y60 toward +X. ) |
G01 X100. | ( Leads out along the extension of the wall, already clear of the material. ) |
G01 G40 X120. | ( Cancels compensation in a linear move and clear of the part. ) |
G00 Z50. M09 | ( Retract in Z and coolant off. ) |
G91 G28 Z0. M05 | ( Z to the reference point and spindle stop. ) |
G90 M30 | ( Back to absolute and end. ) |
The direction is defined looking at the active plane from the positive side of the axis that is missing: in G17 from +Z downward, in G18 from +Y and in G19 from +X. In milling that matches what you see standing in front of the machine looking at the table, so hardly anyone gets G17 wrong. G18 is a different story: the normal on-screen view of an XZ plane, with X to the right and Z up, is the view from -Y, that is, the opposite one, and that is why the same arc looks like it turns the other way. On a lathe you add to that the fact that on rear turret machines positive X points to the other side.
R is short and convenient, and for corner radii and ordinary corners it is perfect. The problem shows up with big arcs: for one radius and the same two points there are two possible arcs, the short and the long one, and the only thing telling them apart is the sign of R, positive for the short one and negative for the long one. Near 180 degrees the center calculation turns unstable, because an error of a micron in the end point moves it a long way, so semicircles get written with I J K. And for a full circle R is no use at all: the end point matches the start point and defines nothing.
If you add the third axis coordinate to the arc, the control interpolates the arc in the plane while it moves that axis proportionally: that is helical interpolation, and it is what lets you open holes bigger than the cutter, thread mill, or drop into a circular pocket without plunging. The lead of the helix is how far Z drops in each full turn. On a lathe, G02 shows up mostly in corner radii and ball noses inside the G18 plane, with I and K or, more usually, with R, and always with tool nose radius compensation set up properly.
Look at the active plane from the positive side of the axis that does not take part. In G17, stand over the part looking down: if the arc turns the way the hands of a clock do, it is G02. If the plane is G18 or G19, that view is not the one on the screen, and that is where everybody gets it wrong.
On Fanuc, Haas and most ISO controls they are incremental from the start point of the arc toward the center, and they stay that way even when the program is in G90. They only change if somebody turns G90.1 on, a mode hardly anyone uses and that is best left alone.
R for arcs clearly smaller than 180 degrees: it is shorter and it reads better. I and J for semicircles, for arcs over 180 degrees and always for full circles. If the arc comes out of a CAM system the post processor already picks for you, normally I J.
Yes, but only with I and J: you program the center and leave the end point the same as the start point, or simply do not write X and Y at all. The control then goes all the way around. With R it is impossible, because there is no way to know which circle you mean.
Because the control checks that the distance from the center to the start point and to the end point match within a very small tolerance, and they do not. The usual causes are rounding CAD coordinates, flipping the sign of an I or a J, or hand editing the end point after the arc was worked out.
CNC IDE: editing with G/M tooltips, line inspector, conversion between controls and 2D/3D toolpath.
CNC Alarms and Solutions Guide. Enter the error code or symptom to find the cause and how to repair it at the machine.
Estimate CNC turning and milling cycle time from G-code. Calculate parts per hour with a breakdown of cutting, rapids, canned cycles and tool changes.