The order of execution of items on a line is defined not by the position of each item on the line, but by the following list:

• the entire line is skipped if it starts with a forward slash / and the block delete toggle is active
• comments started with ( or ;
• if N is the first letter of a line the following number is interpreted as line number
• when a subroutine declaration is found (example O1001) the remaining part of the line is allowed only to be a comment.
• control flow statements like WHILE,IF
• set feed rate mode G93, G94
• set feed rate F
• set spindle speed S
• I/O handling: M62, M63, M66
• change tool: M6 if user tool change macro is disabled, M61, M106
• spindle on or off: M3, M4, M5
• coolant on or off: M7, M8, M9, M17, M18
• M48, M49
• M109, M120
• dwell G4
• set active plane: G17, G18, G19
• set length units: G20, G21
• cutter radius compensation on or off: G40, G41, G42
• cutter length compensation on or off: G43, G49
• coordinate system selection: G54, G55, G56, G57, G58, G59, G59.1, G59.2, G59.3
• set path control mode: G61, G61.1, G64
• set distance mode: G90, G91
• set arc mode: G90.1, G91.1
• set retract mode: G98, G99
• non modal G-codes: G10, G28, G28.1, G30, G30.1, G52, G92, G92.1, G92.2, G92.3
• scaling: G50, G51
• rotation: G68, G69
• motion: G0, G1, G2, G3, G9, G76, G80
• stop: M0, M1, M2, M30, M47
• control flow statements like GOTO
• subroutines and macros: M98, M6 only if user tool change macro is enabled

Some codes require to be the only G/M codes in the line, they are: G65, G100, user defined m codes and user defined g codes