pilot drill macro

[lucas hart]

I am running a Doosan 6300 with a Fanuc B control. In our drilling operations, it is recommended to use a pilot drill or a reduced RPM and feedrate until drill is engaged in hole at twice its diameter. That means a lot of manual code writing for each hole. Has anybody seen a macro that incorporates this in one macro, the lower RPM to a programmed Z depth at a reduced feed then up RPM to recommended speed and increase feed to recommended rate to full Z depth without a peck cycle. Is there something out there where I could just plug in my X, Y and Z numbers and the macro would adjust RPM and feed? Thanks for any help, Lucas

[fordav11]

writing a macro would be fairly simple but you could write the G code once and then copy/paste using a PC? writing programs on a PC is much faster anyway.

its not really much extra code.....

G0 X0 Y0 Z2.0
G1 Z-5.0 F100.0 S500 <-- extra line
G1 Z-100.0 F200.0 S1000
G0 Z2.0
etc


Fanuc B? You mean Fanuc 6, 10, 12, 15, 16, 18, 21 etc. Model B.....

and you have macro enabled on your control right?


well there is a G81-like Modal (G66) macro in all of the Fanuc manuals and I like a challenge so.....

See the attachment for the original code. Note there are a couple of bugs in the manual.
The G code and macro code is right but it shows X Y in the G66 line in the explanation calling format section.
In later manuals X Y has been removed from the G66 line. This is correct. You could put an X and Y on the G66 line but they are ignored because they are passed to the macro as arguments and the macro has nothing in it to make use of #24 (X) or #25 (Y)


I only added H = pilot feed (#11), W = pilot Z position (#23), Q = pilot speed (#17), S = normal speed (#19)
The added bits are in RED.


O0001;
G28 G91 X0 Y0 Z0;
G92 X0 Y0 Z50.0;
G00 G90 X100.0 Y50.0;
G66 P9110 Z–20.0 R5.0 F500 H250 W-5.0 Q500 S1000;
G90 X20.0 Y20.0;
X50.0;
Y50.0;
X70.0 Y80.0;
G67;
M30;


O9110;
#1=#4001; . . . . . . . . . . . . . . Stores G00/G01.
#3=#4003; . . . . . . . . . . . . . . Stores G90/G91.
#4=#4109; . . . . . . . . . . . . . . Stores the cutting feedrate.
#5=#5003; . . . . . . . . . . . . . . Stores the Z coordinate at the start of drilling.
G00 G90 Z#18; . . . . . . . . . . . . Positioning at position R
G01 Z#23 F#11 S#17; . . . . . . . Feed to position W with Feed H and Speed Q
G01 Z#26 F#9 S#19; . . . . . . . . Feed to position Z with Feed F and Speed S
IF[#4010 EQ 98]GOTO 1; . . . . . Return to position I
G00 Z#18; . . . . . . . . . . . . . . . Positioning at position R
GOTO 2;
N1 G00 Z#5; . . . . . . . . . . . . . Positioning at position I
N2 G#1 G#3 F#4; . . . . . . . . . . Restores modal information.
M99;

[lucas hart]

Yes, macros are enabled on the machine. The controller is Fanuc 18i model.

[fordav11]

ok his should work. if you try the above on your machine please let us know if it works like you need it to.
it can be modified if necessary.