Siemens CNC | G70 and G71 Codes | Inch - Metric Conversation


G70 and G71 Codes Introduction

If workpiece dimensions that deviate from the base system settings of the control system are present (inch or mm), the dimensions can be entered directly in the program with G70 and G71 codes. The required conversion into the base system is performed by the control system.

G70 and G71 Codes Format

G70 : Inch dimensions
G71 : Metric dimensions
G700 : Inch dimensions, also for feedrate F
G710 : Metric dimensions, also for feedrate F

Inch / Metric Conversation Example

N10 G70 X10 Z30 ; Inch dimensions
N20 X40 Z50 ; G70 continues to act
N80 G71 X19 Z17.3 ; metric dimensioning from this point on

Things to Know

Depending on the default setting you have selected, the control system interprets all geometric values as either metric or inch dimensions. Tool offsets and settable work offsets including their display are also to be understood as geometrical values; this also applies to the feedrate F in mm/min or inch/min. The default setting can be set via machine data.

G70 or G71 evaluates all geometric parameters that directly refer to the workpiece, either as inches or metric units, for example:

  • Positional data X, Y, Z, … for G0,G1,G2,G3,G33, CIP, CT
  • Interpolation parameters I, J, K (also thread pitch)
  • Circle radius CR
  • Programmable work offset (TRANS, ATRANS)
  • Polar radius RP

All remaining geometric parameters that are not direct workpiece parameters, such as feedrates, tool offsets, and settable work offsets, are not affected by G70/G71.

G700/G710 however, also affects the feedrate F (inch/min, inch/rev. or mm/min, mm/rev.).