2.8 Feedrate: G94,G95,G96,G97

The feed F is the path velocity and represents the value of the geometric sum of the velocitycomponents of all axes involved. The dimension unit for the F word is determined by G functions:

1. G94 F as the feedrate in mm/min

2. G95 F as feedrate in mm/rev of the spindle

3. G96 constant cutting rate ON

4. G97 constant cutting rate OFF

G94 and G95 are used to define the feedrate unit, G94 is the default command, G95 is meaningful only when the spindle rotation.

Example:

N10 G94 F310                                            ;Feedrate 310 mm / min.

…

N110 S200 M03                                          ;Spindle rotation

N120 G95 F1.5                                           ;Feedrate 1.5 mm / rev.

Note:

F instruction does not have to be with G94/G95 in the same block, as long as be defined before or in the block with G01, G02, G03:

N10 G94 F200

N20 G01 X20

and

N10 G94

N20 G01 X20 F200

It is equivalent.

 Note

The programmed value of F must be greater than zero, otherwise an alarm is occured. If F value is not programmed in a program, F is considered as zero, axis will not move.

Explanation:

1. For turning system, the G94, G95 also contains the functions G96, G97 for the constant cutting rate.

2. With activated G96 function, the spindle speed is adapted to the currently machined workpiece diameter (transverse axis) such that a programmed cutting rate S remains constant on the tool edge (spindle speed multiplied with the diameter = constant).

3. The S word is evaluated as the cutting rate as of the block with G96. G96 is modally effective until cancellation by another G function of the group (G94, G95, G97).

 Fig.2.30 Constant cutting rate

 Programming:  

G96 S… LIM=… F…                        ; Constant cutting speed ON

G97                                                 ; Constant cutting speed OFF

S                                                       ; Cutting rate, m/min

LIM=                                                ; Upper limit speed of the spindle with G96 effective

F                                                       ; feedrate in mm/rev of the spindle,as for G95

Note

During machining from large to small diameters, the spindle speed can increase significantly. In this case, it is recommended the upper spindle speed limitation LIMS=... . LIMS is only effective with G96 and G97. LIM value is not permitted to go beyond the limitation set in machine data, when it is not set, the value is zero.

The function "Constant cutting rate" is deactivated by G97. If G97 is active, a programmed S word is given in RPM as the spindle speed .

Example:

N10 S600 M03                                            ; Spindle's direction of rotation

N20 G96 S120 F0.5 LIM=2500                      ; Activate constant cutting speed, 120 m/min, speed limit 2,500 r.p.m.

N30 G01 F0.2 X32 Z…                               ; Feedrate 0.2 mm/revolution, change in speed

……

N180 G97 S400                                          ; Deactivating constant cutting rate, new spindle speed, r.p.m.

Explanation:

1. The G96 function can also be deactivated with G94 or G95 (same G group).

2. When G00 instruction is active in G96 mode, the spindle speed will not be adapted to the X axis movement.

3. After M05/M19/SPOS instructions are programmed in G96 mode, when movement instruction is programmed, feed axs stop.

4. After G94/G95/G97 instead of G96, the value of S and F need to be reprogrammed