Structure of an NC program

The structure of an NC program explained: program start, tool call, approach, machining and program end – with a commented G-code example from CAM output.

In most cases, NC code follows a clear structure – especially when it was generated by CAM software. Depending on the section, the program contains different information and instructions: from the program header through tool calls to the actual machining blocks.

The following graphic shows what such a structure looks like:

The structural elements at a glance

The individual structural elements contain different information:

• Program start
  • Program name
  • Program header
  • Additional information
• Tool call
  • Tool information
  • Spindle speed
• Operation start
  • Structuring element (comment, section marker)
  • Speed change
  • Machining configuration
    • Main spindle / counter spindle
    • Driven tools
• Approach
  • Tool length compensation
  • Work offset
  • Tilting
  • Coolant
  • Machining configuration
    • RTCP
    • Transmit
    • Unclamping / clamping the rotary axes
• Machining
  • Feed rate
  • Radius compensation
  • Geometry information
  • Machining cycles
• Retract
  • Retract to safe height
  • Coolant off
• Program end
  • Spindle and coolant stop
  • Program end command (M30)

Example: a CAM-generated program skeleton

This is what the skeleton of a typical CAM-generated milling program looks like. The comments in parentheses map each block to the structural elements in the graphic:

%
O1000                    (PROGRAM NAME)
G90 G94 G17 G21          (SAFETY BLOCK: ABSOLUTE, MM/MIN, XY PLANE, METRIC)
T1 M6                    (TOOL CALL: LOAD TOOL 1)
S8000 M3                 (SPINDLE CLOCKWISE AT 8000 RPM)
G54 G0 X10 Y10           (APPROACH: WORK OFFSET G54, RAPID TO START POSITION)
G43 H1 Z50               (ACTIVATE TOOL LENGTH COMPENSATION, SAFE HEIGHT)
M8                       (COOLANT ON)
G1 Z-2 F300              (FEED DOWN TO CUTTING DEPTH)
G1 X60 F800              (MACHINING: LINEAR MOVE AT CUTTING FEED)
G1 Y40
G1 X10
G0 Z50                   (RETRACT TO SAFE HEIGHT)
M9                       (COOLANT OFF)
M5                       (SPINDLE STOP)
M30                      (PROGRAM END)
%

Each subsequent operation repeats this pattern: tool call, approach, machining, retract. Only after the last operation does M30 end the program.