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.
M30 ends the program: the control stops the feed, normally stops the spindle and the coolant, and puts itself back on the first block, ready to machine the same part again. It is the last line of practically every milling and turning program. Its relative M02 also ends, but classically it does not rewind. What is worth being clear about is that M30 is not a safety block: retracting the tool, stopping the spindle and shutting the coolant have to be written before it.
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
M30End of program and rewind to the first block. What modal state is left afterwards (G90 or G91, the active work offset, the plane, the units) is decided by machine parameters, so you cannot take it for granted that the control goes back to G90 on its own.
Haas
M30It ends, rewinds and also increments the two parts counters of the control, which is how a production run is tallied. With Setting 118 on, an M99 in the main program increments those counters too.
Siemens 840D / 828D
M30M30 and M2 end the program the same way on most Siemens machines. M17 is the end of a subprogram, not of a program. The state the control is left in at the end is defined in the machine data.
Heidenhain TNC (Klartext)
END PGM PIEZA1 MMIn Klartext the end of the program is the END PGM line, which the control itself writes when the program is created. M30 is accepted in ISO format programs and on many TNCs it can be written next to the final line.
Machines with automation
M30On machines with a bar feeder, a robot or a pallet changer, the M30 can also be the signal that triggers the next cycle. When parts have to be chained with no intervention, plenty of shops use an M99 in the main program instead.
| Letter | What it sets | Unit |
|---|---|---|
| No address letters | M30 goes alone in its block. It takes no arguments of any kind and it is usually the last line of the file, followed by the end of program character where the control uses one. | no units |
| Parts counter | It is not programmed, but it is part of what it does: many controls add a part to the counter every time they run an M30. It is the number you look at to know how many of the run are done. | parts |
| Modal state after the M30 | Which codes are left active after the end (absolute or incremental, work offset, units, plane) depends on control parameters. It is a machine setting, not a property of the code. | machine setting |
The complete closing block of a milling program. The M30 is the last line, but what makes the ending safe is the blocks before it: cancelling cycles and offsets, shutting the coolant, retracting in Z, sending the axes to the reference point and stopping the spindle. This block is copied as it stands onto the end of any program and it avoids half the scares of the next start.
G99 G81 X120. Y40. Z-12. R3. F220 | ( Last hole of the last operation: the program reaches the close with a canned cycle active and the coolant running. ) |
G80 G40 | ( Cancels any canned cycle and cutter compensation. Finishing with G41 active means the next tool starts offset by half a cutter. ) |
G00 Z50. M09 | ( Retracts the tool in Z and shuts the coolant, with the machine still under program control. ) |
G91 G28 Z0. M05 | ( Z to the reference point in incremental and spindle stop. Under G90 this block would drop to the part Z0 first, which is the face. ) |
G91 G28 Y0. | ( Sends Y to the reference point as well to leave the table out so the next part can be loaded comfortably. On some machines a G53 to a particular position is preferred. ) |
G49 | ( Cancels the length offset with the machine already at the reference point, to leave the control in a predictable state. ) |
G90 | ( Puts the control back in absolute. Whether the M30 restores it depends on a parameter, and starting the next program in incremental is a crash. ) |
M01 (REVISAR ACABADO CADA 10 PIEZAS) | ( Optional stop before the close: if the operator has it switched on, he can look at the part without editing the program. ) |
M30 | ( End of program. The control goes back to the first block, adds a part to the counter and is ready to start again. ) |
It does three things: it stops execution, it leaves the pointer on the first block so cycle start runs the same part again and, on most machines, it cuts the spindle and the coolant and increments the parts counter. It does not do what plenty of people assume: it does not retract the tool, it does not send the axes to the reference point, it does not open the door and it does not guarantee that cutter compensation, length offset or incremental mode are cancelled. All of that is machine parameters or blocks you have to write. M30 is the full stop at the end of the sentence, not the summary.
The sequence that works on any machine is short: cancel the cycle and cutter compensation with G80 and G40, retract in Z and shut the coolant with M09, go up to the reference point with G91 G28 Z0. and stop the spindle with M05, cancel the length with G49, go back to G90 and finish with M30. If the machine has to end up in a comfortable loading position, you add a G53 to that position or a G28 in Y. Writing that block is not fussiness: it is what lets the next program start from a known state instead of inheriting the last one.
In a run, the M30 is also the point where the control adds a part. Those counters are there to cut production at a quantity, to call for an insert change every so many parts or simply to know how many you have done. On automated machines, with a bar feeder or a robot, the end of the program can chain straight into the next part: some shops handle it with the signal the M30 itself sends the automation and others replace the M30 with an M99 that restarts the program in a loop, normally with the block delete slash so it can be broken.
Both end the program. The classic difference is that M30 rewinds the pointer to the first block and leaves the control ready to repeat the part, while M02 ends where it is. On many modern controls they behave the same, but since that depends on the machine, the sensible thing is to use M30 every time.
On most machines yes, because the PLC provides for it. Even so it is not an obligation of the code, and it depends on the builder. The shop habit is to write M05 and M09 in the closing blocks, which also makes clear to whoever reads the program what state is expected at the end.
It depends on control parameters. There are machines set up to return to the initial state after end of program and others that keep the modals. Since you cannot know without looking at the machine, the practical answer is to cancel what matters by hand with G40, G49 and G90 before the M30.
It is not compulsory, but it is strongly recommended: leaving Z up and the table in a comfortable position lets you load the next part without fighting the tool, and it means the next program always starts from the same place. G91 G28 Z0. is enough in most cases.
By replacing the M30 with an M99 in the main program, which restarts from the first block. It only makes sense on machines where the next part comes in on its own, with a bar feeder or with automation, and it should be written with the block delete slash in front so the operator can break the loop from the panel.
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.