96-8000 165
G CODES
June 1999
G10 Examples:
G10 L2 P1 G91 X6.0 {Move coordinate G54 6.0 to the right.};
G10 L20 P2 G90 X10. Y8. {Set work coordinate G111 to X10.0 ,Y8.0};
G10 L10 G90 P5 R2.5 {Set offset for Tool #5 to 2.5.};
G10 L12 G90 P5 R.375 {Set diameter for Tool #5 to 3/8ths.};
CIRCULAR P OCKET M ILLING (G12, G13)
There are two G codes that will provide for pocket milling of a circular shape. They are different only in which
direction of rotation is used. Both are only functional in the default XY circular plane selection mode (G17).
G12 Circular Pocket Milling Clockwise Group 00
*D Tool Radius Or Diameter Selection
I Radius Of First Circle (Or Finish If No K)
K Radius Of Finished Circle (If Specified)
L Loop count for repeating deeper cuts
Q Radius Increment (Must Be Used With K)
F Feed Rate in inches (mm) per minute
Z Z depth of cut or increment
*In order to get the exact programmed circle diameter, the control uses the selected D code tool size.
If this compensation is not desired, program D0.
This G Code implies the use of G42.
The tool must be positioned at the center of the circle either in a previous block or in this block using X and Y.
The cut is performed entirely with circular motions of varying radius. To remove all the material within the circle
use an I and Q value less than tool diameter and a K value equal to circle radius. To cut circle radius only use
an I value set to circle radius and no K or Q value. G12 belongs to Group zero and thus is non-modal. If G91
(incremental) is specified and an L count is included, the Z increment is repeated Ltimes at the F feed rate.
G13 Circular Pocket Milling Counterclockwise Group 00
This G Code implies the use of G41 and is otherwise similar to G12. G13 belongs to Group 00 and thus is
non-modal.
To Next Page
Loading...
Need help?
General
