Fanuc G71 Turning Cycle
G71 turning cycle is used for rough-material removal from a cnc lathe component. G71 turning cycle makes large diameter cutting easy. Cutting can be done in simple straight line or a complex contour can also be machined very easily.
Through G71 turning cycle parameters cnc machinists can control
- Depth of cut.
- Retract height.
- Finishing allowance in x-axis and z-axis.
- Cycle cutting-feed, spindle speed.
G71 U... R... G71 P... Q... U... W... F... S...
|U||Depth of cut.|
|P||Contour start block number.|
|Q||Contour end block number.|
|U||Finishing allowance in x-axis.|
|W||Finishing allowance in z-axis.|
|F||Feedrate during G71 cycle.|
|S||Spindle speed during G71 cycle.|
G71 Turning Cycle Overview
- G71 turning cycle cuts the whole contour repeatedly which is given in P Q blocks.
- Depth of every cut can be controlled by first-block U value.
- Second-block U W are the finishing allowances which can be given if you want to make a finish cut with G70 finishing cycle.
- F is cutting feed and S is spindle speed (given in second-block) which are used during G71 turning cycle.
Note – The F and S given inside P Q block will not be used during G71 turning cycle, they are used with G70 finishing cycle if later called.
G71 Turning Cycle Working
N60 G71 U10 R10 N70 G71 P80 Q90 U3 W0 F0.25 N80 G00 X60 N90 G01 Z-75
When G71 turning cycle is run the whole operation will be done in following sequence,
1 – Tool will move in x-axis U (depth of cut) deep with programmed feed from starting-point.
2 – Tool will travel with feed in z-axis (destination point in z-axis is given in P Q blocks )
3 – Tool rapidly retracts R amount in both x-axis and z-axis (at 45 degrees).
4 – Tool rapidly travel in z-axis to start-point
5 – Tool rapidly moves to last cut depth.
6 – Tool moves with feed in x-axis U deep (first-block U depth of cut).
7 – Tool with feed moves in z-axis (destination point given in P Q blocks).
8 – Tool rapidly retracts in x-axis and z-axis R amount (45 degrees).
9 – Tool rapidly moves to start-point only in z-axis.
This whole sequence of operation keep on going, until the destination point in x-axis is met.
If finishing allowance is given tool will not make the exact diameter and length given in P Q blocks but will leave that much allowance, This finishing allowance can be later machined by calling G70 finishing cycle.
Fanuc G71 Example
Here is a cnc part-program which shows how G71 turning cycle can be used, this is the program for the drawing given above
N50 G00 X106 Z5 M3 S800 N60 G71 U10 R10 N70 G71 P80 Q90 U3 W0 F0.25 N80 G00 X60 N90 G01 Z-75
In this program G71 turning cycle will keep repeating the contour given inside P Q blocks shown below
N80 G00 X60 N90 G01 Z-75
These two cnc program blocks tell us that we want to remove material till X60 deep and in Z-75 in length.
The depth of cut is given in first-block U10 retract amount is also given R10.
Finishing allowance in x-axis is U3 but there is no finishing allowance given in z-axis W0.
G70 Finishing Cycle
If you programmed G71 turning cycle with finishing allowances then that finish allowances can be removed with G70 finishing cycle.
G70 finishing cycle repeats the whole contour the G71 way, but in just one-cut removing the finishing allowances.
Why Use G70 Finishing Cycle
As material can be removed with G71 turning cycle, but if you want a different cutting-feed and spindle speed for the last cut, then it is recommended that you use G70 finishing cycle.
G70 finishing cycle use F and S values which are given inside P Q programmed blocks. (G71 use F S values which are given inside G71 second block.)
Fanuc G70 Example
N50 G00 X106 Z5 M3 S800 N60 G71 U10 R10 N70 G71 P80 Q90 U3 W0 F0.25 N80 G00 X60 N90 G01 Z-75 F0.15 N100 G00 X200 Z100 N110 G92 S1200 N120 T3 G96 S150 M03 N130 G00 X106 Z5 N140 G70 P80 Q90 N150 G00 X200 Z100 N160 M30
G70 G71 Example
O0004 G00 X200 Z10 M3 S800 G71 U2 R1 F200 G71 P80 Q120 U0.5 W0.2 N80 G00 X40 S1200 G01 Z-30 F100 X60 W-30 W-20 N120 X100 W-10 G70 P80 Q120 M30