12. COMPENSATION FUNCTION
By specifying G39 in offset mode during cutter compensation C, corner
circular interpolation can be performed. The radius of the corner circular
interpolation equals the compensation value.
In offset mode
When the command indicated above is specified, corner circular
interpolation in which the radius equals compensation value can be
performed. G41 or G42 preceding the command determines whether the
arc is clockwise or counterclockwise. G39 is a one–shot G code.
When G39; is programmed, the arc at the corner is formed so that the
vector at the end point of the arc is perpendicular to the start point of the
When G39 is specified with I, J, and K, the arc at the corner is formed so
that the vector at the end point of the arc is perpendicular to the vector
defined by the I, J, and K values.
In a block containing G39, no move command can be specified.
Two or more consecutive non–move blocks must not be specified after a
block containing G39 without I, J, or K. (A single block specifying a
travel distance of zero is assumed to be two or more consecutive
non–move blocks.) If the non–move blocks are specified, the offset
vector is temporarily lost. Then, offset mode is automatically restored.
Use with edge machining or startup machining is not supported.
D Corner circular
D G39 without I, J, or K
D G39 with I, J, and K
D Move command
D Non–move command
D Use with edge machining
or startup machining