What Is G Code and Mcode in CNC Machine Control

• 1
  Key takeaways
• 2
  How G Code and Mcode in CNC Machine Work Together
• 3
  The G Codes That Cover Most Milling and Turning Work
• 4
  M Codes: Spindle, Coolant, Tool Change and Program Control
• 5
  Why Modal State Causes Most Programming Errors
• 6
  What Code Choice Changes on the Machine
• 7
  Reading a CNC Program Block by Block
• 8
  G Code vs M Code: What Each One Controls

A CNC program is a list of blocks. Each block is one line of text, and most controllers read it word by word: a letter address plus a number. G words handle motion and geometry. M words handle machine state. X, Y, Z, I, J, K, F, S and T carry the values those words need.

The split is not arbitrary. Motion is something the controller can calculate and verify in advance. Machine state is a physical action: a spindle ramping to 12,000 rpm, a coolant pump starting, an automatic tool changer swinging an arm. The controller has to sequence those actions around the motion so nothing collides.

That is why a typical block looks like N120 G01 X45.0 Y12.5 F250 M08. The tool moves in a straight line at 250 mm/min while coolant turns on. The M08 does not wait for the move to finish in most controls. It fires in parallel, because flooding the cut early is better than flooding it late.

The two families are also standardized differently. G and M codes follow ISO 6983, but every builder adds its own codes on top. A Fanuc M code list is not the same as a Siemens list. When a shop moves a program between machines, the post-processor has to be rebuilt, not just copied.

• 1
  Word address formatLetter plus number, one block per line, no separators required.
• 2
  Two code familiesG for motion and offsets, M for machine functions and program flow.
• 3
  Parallel executionMany M codes run while the axis is still moving.
• 4
  Vendor extensionsProbing, high-speed look-ahead and pallet change codes vary by builder.

G00 is rapid positioning. The machine moves at its fastest traverse rate to a point, usually above the part. G01 is a straight feed move at the programmed feed rate. G02 and G03 are circular interpolation, clockwise and counterclockwise. Between them, these four codes describe nearly every path a machinist cuts.

Offsets come next. G54 through G59 set the work coordinate system, so the program's zero point can sit at a corner of the stock instead of machine zero. G41 and G42 apply cutter radius compensation, letting the programmer define the part geometry and let the control shift the path by the tool radius. G43 applies tool length offset from the tool table.

Canned cycles compress repetitive drilling and tapping. G81 is a simple drill cycle. G83 pecks in steps, which clears chips in deep holes. G84 taps. On a lathe, G71 and G70 handle rough and finish turning passes. One G83 block with a Q value can replace 40 lines of G01 and G00.

High-speed machining options change how these codes execute. Look-ahead buffers thousands of blocks and smooths corners so the machine does not stop at every junction. Without it, a complex 3D surface program runs at a fraction of the programmed feed. With it, the same program holds tolerance and cuts cycle time.

• 1
  G00 / G01Rapid traverse and linear feed, the two most common motion codes.
• 2
  G02 / G03Circular interpolation with I, J, K center offsets or an R radius.
• 3
  G41 / G42Cutter compensation left or right of the path direction.
• 4
  G81 / G83 / G84Drill, deep-hole peck drill and tap cycles.

M03 starts the spindle clockwise. M04 runs it counterclockwise. M05 stops it. The speed comes from the S word in the same block, so M03 S8000 spins at 8,000 rpm. On a lathe, M03 usually means the spindle turns so the top of the insert cuts, which is why the direction matters more than on a mill.

M06 is a tool change. On machines with an automatic tool changer, M06 T07 sends the carousel to pocket 7 and swaps it into the spindle. The controller also reads the tool length offset from the table at that point, so the next G43 does not need the length typed out.

Coolant is M07 for mist, M08 for flood and M09 to stop. The choice is not cosmetic. Flood coolant removes heat from deep pockets and flushes chips. Mist is common in aluminum at high spindle speeds where flood would splash and where chip evacuation is already good. On titanium and stainless, flood is the default because heat stays in the cut.

Program flow uses M00 for a stop, M01 for an optional stop, M02 for program end without reset and M30 for program end with reset. M30 is the one most shops put at the bottom of a file. It rewinds to the top and clears modal state, ready for the next part.

• 1
  M03 / M04 / M05Spindle forward, reverse and stop.
• 2
  M06Automatic tool change, usually paired with a T word.
• 3
  M07 / M08 / M09Mist coolant, flood coolant, coolant off.
• 4
  M30End of program with rewind and modal reset.

Modal means the code stays in effect after the block that called it. If line 50 says G01 and line 51 only has X and Y, the control still feeds at the same rate along a straight line. This saves thousands of characters in a long program, but it also means a single stale G code can ruin a part.

The classic case is a missed G00. A programmer leaves out the rapid move after a cut and the next block feeds at cutting speed into the stock. Or a G41 stays active after a contour and the next pocket is offset by the tool radius. Both errors trace back to modal state that nobody cancelled.

Safety blocks exist for this reason. Many shops end a toolpath with G40 to cancel cutter compensation, G49 to cancel tool length offset and G80 to cancel canned cycles. It costs three short lines. It prevents a scrap part that costs far more than the programming time saved.

On a 5-axis machine, the problem compounds. G43.4 and G43.5 for tool center point control change how the rotary axes are calculated. If one of those modes stays active into the next operation, the post-processor output no longer matches the machine's interpretation and the tool can drive into the fixture.

• 1
  Modal G codesG00 to G03, G40, G41, G43, G80 all persist across blocks.
• 2
  Non-modal codesG04 dwell and G53 machine coordinate move apply once.
• 3
  Reset habitEnd each operation with G40, G49 and G80.
• 4
  5-axis cautionCancel TCP modes before switching to a new operation.

Programming decisions show up in three places: tolerance, cycle time and tool life. A trochoidal path with a small radial depth of cut keeps the tool engaged at a steady angle, which holds ±0.005 mm on a deep pocket and extends carbide life. A conventional full-width pass may finish faster in theory and fail in practice on the same feature.

Cycle time moves with feed rate and rapid distance. Raising feed from 250 to 400 mm/min helps only if the tool and the setup can take it. On a thin-wall aluminum part, the same change causes chatter and forces a second finishing pass. The code is correct. The physics is not.

Tool life is a code question too. G83 peck drilling with a Q value of 3 mm clears chips and avoids re-cutting on deep holes. A G81 straight drill on the same hole loads the flutes with chips and burns the tip. The material and depth decide which cycle is right, not habit.

At GreatLight, 127 high-precision CNC machines run programs across 3-axis, 4-axis, 5-axis and mill-turn centers. The largest travel is 4,000 × 400 × 150 mm. Programming is matched to the machine that will cut the part, because a program that runs clean on one control can behave differently on another.

• 1
  Toolpath shapeTrochoidal paths hold tolerance in deep pockets.
• 2
  Feed and speedHigher feed helps only when the setup is rigid enough.
• 3
  Canned cycle choicePeck drilling protects tool life in deep holes.
• 4
  Machine matchingPrograms are posted for the specific control and machine.