Contents - Index - Previous - Next

This cycle is used when NC code is created manually.

The picture shows a billet whose end is to be machined flat and true true. This facing process is often the first thing done when machining a part.

A G0 command brings the tool to starting position P0. The G88 command will make the tool move in a series of rectangular paths cutting material radially until the tool tip reaches target point P1 where the cycle ends. Cutting movements will be at the cutting feed rate. All other movements will be at rapid traverse rate.
 
The best way to appreciate the cycle is to get WELturn to simulate the G88 illustration below. Copy everything between the % symbols, including the % symbols, into UNCONVERTED WINHELP MACRO:!EP(`C:\\windows\\notepad.exe',0)Notepad. Save the file in C:\WELturn\Turndata with the extension .cnc

Go into WELturn and run the file in simulation mode only: do not try to machine anything. Observe the path of the tool as it executes the cycle.

G88 illustration (metric)
%
*Billet diameter 25
N10 T1
N20 S950
N30 G0 X26 Z5
N40 G0 X26 Z0
N50 G88 X0 Z-20 F100 H2
%

Line N40 locates P0.

In line N50, X0 Z-20 locate P1. When the tool reaches this point the cycle ends. The tool then moves to the right by the width of the previous cut and stops. If a shoulder had been cut this final movement would clean the shoulder.

The full format of the G88 command is:

N(line number) G88 X(co-ord of P1) Z (co-ord of P1) F(cutting feed rate) H(depth of cut)

For example:
N40 G88 X-0.4 Z-3 F100 H0.5

Notes

the X co-ordinate in a G88 line is the diameter at P1. To completely face off the end of a billet, as in the example above, X0 can be used to locate P1. However, because the tool tip has a radius of 0.4mm, a pip will be left on the end of the material. This is avoided if a value of X-0.4 is used instead;
·