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.
In the canned cycles of a milling machine, G98 and G99 decide how high the tool comes out after each hole: with G99 it goes back only as far as the R plane and with G98 it climbs to the initial plane, which is the Z the axis was at when the cycle started. G99 saves cycle time and G98 is what saves clamps, vise jaws and steps. Careful on a lathe: on Fanuc A system lathes and on Haas lathes, G98 and G99 are not return planes but feed modes, per minute and per revolution.
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.
Fanuc (milling)
G99 G81 X20. Y20. Z-18. R3. F200Both are modal and belong to the same group, so you can slot them in between one hole and the next: it is enough to write G98 in the block of the hole after which you have to cross an obstacle. The power up state on most controls is G98.
Haas (milling)
G99 G81 X20. Y20. Z-18. R3. F200Identical to Fanuc. Haas adds Setting 52 (G83 Retract Above R), which changes how far the peck cycle retracts above the R plane, and that stacks on top of whatever G98 and G99 decide.
Fanuc / Haas (turning)
G99 G01 X40. Z-30. F0.25On a lathe they have nothing to do with planes: G99 is feed per revolution and G98 feed per minute. It is the same pair of codes with two completely different meanings depending on the machine, and mixing them up is a classic when you move from the mill to the lathe.
Siemens 840D / 828D
CYCLE81(100, 0, 3, -18)Siemens uses neither G98 nor G99 in cycles: the two heights are parameters of the cycle itself, RTP (retract plane, the first one) and RFP (reference plane). With MCALL active, the return between positions is made to the retract plane.
Heidenhain TNC (Klartext)
CYCL DEF 200 TALADRADO Q200=+3 Q204=+100It goes by parameters here too: Q200 is the set-up clearance, which acts as the R plane, and Q204 is the second set-up clearance, which acts as the initial plane for clearing obstacles. The control decides which to use depending on whether there is a collision risk between points.
| Letter | What it sets | Unit |
|---|---|---|
| G98 / G99 | Modal selector of the return plane in milling. They take no arguments and stay active until the other replaces them or until a reset. | modal, no units |
| Initial plane | It is not written: it is the Z coordinate the axis was at just before the first block of the cycle. Start the cycle from Z2 and the initial plane is Z2, so a G98 climbs no higher than that. | mm / in |
| R | Reference plane of the cycle: the height where the tool switches from rapid to feed and the one it returns to under G99. The usual value is 2 or 3 mm above the face. | mm / in |
| G80 | Cancels the cycle. Until it is written, any block with an X or a Y repeats the hole, and the return is still governed by the active G98 or G99. | modal, no units |
Six holes in a long plate held down by two clamps in the middle. The holes on the left and on the right are in clear ground, but the move from one group to the other crosses over the clamps. That jump is the reason G98 exists, and the example shows exactly which block it has to be written in.
O0098 (SEIS AGUJEROS CON BRIDAS EN MEDIO) | ( Program header. ) |
G21 G17 G40 G49 G80 | ( Millimeters, XY plane and a clean state. ) |
G91 G28 Z0. | ( Z to the reference point in incremental before the change. ) |
T5 M06 | ( 8 mm drill. ) |
G90 G54 G00 X20. Y30. | ( Absolute, work offset and positioning over the first hole. ) |
G43 H05 Z100. M03 S2400 | ( T5 length offset and spindle on. That Z100 is the key to the example: it will be the initial plane, and it is deliberately above the clamps. ) |
M08 | ( Coolant on. ) |
G99 G81 Z-22. R3. F200 | ( First hole. Rapids down from Z100 to Z3, drills to Z-22 and returns to Z3, because G99 is active. ) |
X60. | ( Second hole. The move happens at Z3 and the path is clear. ) |
X100. | ( Third hole, also at Z3. ) |
G98 X140. | ( Fourth hole, the last one before the clamps. On finishing it climbs to the initial plane Z100 instead of staying at Z3. ) |
G99 X220. | ( Fifth hole, now on the other side. The move happens at Z100, which is where the tool was left, so it passes over the clamps; once there it drops to R and goes back to behaving like G99. ) |
X260. | ( Sixth hole, with the path clear again. ) |
G80 G00 Z100. M09 | ( Cancels the cycle before any rapid move and shuts the coolant off. Without the G80, this very block would drill. ) |
G91 G28 Z0. M05 | ( Z to the reference point and spindle stop. ) |
G90 M30 | ( Back to absolute and end. ) |
The initial plane is not programmed in the cycle: it is simply the Z coordinate the axis was at when the first block of the cycle ran. That is why the G43 block with the safe Z is the one that decides, without looking like it, how high a G98 will climb later on. If the program drops to Z5 before starting the cycle, the initial plane is Z5 and writing G98 buys you nothing. The healthy habit is to start cycles from a Z clearly above everything on the table.
G99 is faster because every hole ends two or three millimeters off the face, and on a plate with forty holes the difference is minutes. G98 is used when there is something between two holes taller than the R plane: clamps, nuts, vise jaws, a step in the part itself or a bar stop. Also when the holes are on faces at different heights, or when the move passes over an area already machined with walls in it. The efficient way is not to pick one for the whole cycle, but to slot G98 in only on the blocks where the path is not clear.
On Fanuc lathes with the A code system and on Haas lathes, G98 and G99 are the feed mode: G98 in millimeters per minute and G99 in millimeters per revolution. There are no return planes because lathe cycles handle their own heights with other parameters. On Siemens and Heidenhain the concept exists but does not carry these codes: they are parameters inside the cycle, RTP and RFP on Siemens, Q200 and Q204 on Heidenhain. Before copying a block from one machine to another, look at which control it came from.
The height the tool comes out to after each hole of a canned cycle. With G99 it returns to the R plane, which is usually two or three millimeters off the face. With G98 it climbs to the initial plane, which is the Z the axis had when the cycle started. Both are modal and you can alternate between them from hole to hole.
On most Fanuc and Haas controls the power up state is G98, but that is also a machine parameter and, above all, whichever the previous program left can still be active. Always writing it in the first block of the cycle takes the doubt away and costs nothing.
By writing the new code in the block of the hole concerned, next to the coordinate: G98 X140. drills that hole and comes out to the initial plane. The next block can go back to G99 with no problem, because the move will already have happened at the high level.
No. On Fanuc A system lathes and on Haas lathes they are the feed modes: G98 per minute and G99 per revolution. It is the same pair of codes with a different meaning, so a block copied from a mill to a lathe changes the feedrate instead of the return height.
As codes, no. Siemens defines the two heights inside the cycle with the RTP and RFP parameters, and Heidenhain with Q200 (set-up clearance) and Q204 (second set-up clearance). The concept is identical: a short height to move fast and a high one to clear obstacles.
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.