G70 Finishing Cycle | Contour Finishing

G70 Finishing Cycle

G70 Cycle is a CNC code and used for finish cutting operations (final cleaning cutting) in CNC lathes. G70 code is used to final cutting after any roughing cycles like G71 Turning Cycle, G72 or G73 Cycle.

The G70 cycle is not used alone. It is used after G71 Turning Cycle, G72 Cycle and G73 Pattern Repeating Cycle and follows the same tool path as the used cycle. The G70 CNC code is used if U and W parameters are valued from the second row of G71, G72 and G73 cycles (briefly other roughing cycles).

If “0” is written to U and W in roughing cycles (G71, G72 or G73), the G70 canned cycle is not written at the end of the program. With the G70 canned cycle, chip removal can be done with the tool used in rough turning or with different cutting tool. The G70 command consists of a single line.

G70 Finishing Cycle Format

G70 P… Q… F… S…;


P : First block number of the finishing contour
Q : Last block number of the finishing contour
F : Cutting feedrate (in/rev or mm/rev)
S : Spindle speed (ft/min or m/min)

G70 canned cycle accepts a previously defined finishing contour from either of the three roughing cycles, already described. This finishing contour is defined by the P and Q points of the respective cycles, and is normally repeated in the G70 cycle, although other block number references may be used - be careful here!

For safety, always use the same start point for G70 as for the roughing cycles!

G70 CNC Code Examples

G70 Finishing Cycle with Same Tool

G70 Cycle Example

N5 T0101;
N10 M3 S1800;
N15 G0 X83 Z0 M08;
N20 G71 U1 R1;
N25 G71 P30 Q60 U0.2 W0.1 F0.18;
N30 G1 X50;
N35 G1 Z-2;
N40 G1 X60 Z-23;
N45 G1 Z-48;
N50 G1 X76;
N55 G1 X80 Z-53;
N60 G1 Z-68;
N65 G70 P30 Q60;
N70 G00 X200 Z200 M09;
N75 G28 U0 W0;
N80 M30;

G70 Finishing Cycle with Different Tool

In such a case, we can use the example above exactly. All we need to do is to call the tool that will remove the finish pass with the offset number just above the line N65 where we write the G70 command. So in such a case, between the N60 and N75 lines of the above program would be as follows:

N60 G1 Z-68;
N62 T0303;
N65 G70 P30 Q60;
N70 G00 X200 Z200 M09;
N75 G28 U0 W0;