CNC Drilling and Tapping Commands

Sat, Jun 5, 2010

FAQs, G-Code, Threading and Tapping

Dear Answer Man,

I am converting a program from another brand of machine to our Haas VF-3. The G81 canned cycle utilizes a “K19,” which is the number of times to incrementally move in “X” to drill to the “Z” value. What variable does Haas use for this?

Steve

Dear Steve,

The Haas mill control has a G72 command. This command allows you to drill a series of holes in a straight line. The G72 command may be used with drilling, tapping and boring canned cycles. Use an I value to define the distance, incrementally, between holes, and an L value for number of holes. This line can also be at an angle. You specify the angle of the line of holes with a J command. The J value is the angular starting position, and is always 0 to 360 degrees counterclockwise from the 3 o’clock position. Refer to your Operator’s Manual for more information about using G72 with canned cycles.

Another way to do this is with a G91 (Incremental Positioning) command. Here is a simple program to drill 100 holes in a grid plate using G91, and an L command for the number of times to repeat the G81 drill cycle along the specified axis.

%

O3400 (Drilling grid plate)

T1 M06

G00 G90 G54 X1.0 Y-1.0 S2500 M03

G43 H01 Z.1 M08

G81 Z-1.5 F15. R.1

G91 X1.0 L9

Y-1.0

X-1.0 L9

Y-1.0

X1.0 L9

Y-1.0

X-1.0 L9

Y-1.0

X1.0 L9

Y-1.0

X-1.0 L9

Y-1.0

X1.0 L9

Y-1.0

X-1.0 L9

Y-1.0

X1.0 L9

Y-1.0

X-1.0 L9

G00 G90 G80 Z1.0 M09

G28 G91 Y0 Z0

M30

%

Sincerely, Answer Man

|| More
, , ,