Use of G12/G13 Counter Bore Cycle
When
circle milling, we typically use the G2 or G3 (directional) command
along with a G41 or G42 code (for the cutter compensation) and the I
code to dictate the radius or circle size. You’ll also have to
program the ramp-in and ramp-out move for the end mill.
This sounds complex. The G12/G13 codes can
simplify programming for circle milling. This cycle is a one-line
command that can easily produce a quality bore with a minimum of
programming stress.
The counterbore is machined with an end
mill. The G12 command machines the circle in a clockwise direction
and the G13 in a counter clockwise direction.
Climb milling is preferable to conventional
milling. As climb milling is safer and machining forces are directed
into the machine table, we will focus on the counter clockwise
milling with G13.
To machine a 3.250 size counter bore, let’s
use a 0.750 size end mill. The bore is started with a 1.250 diameter
drilled hole at the center of the bore. Take a look at the program
code to machine the circle.
T1
M6; (0.75 end mill)
G17 G54 X0 Y0 B0;
G43 H1 Z.1 M3 S1018 M8;
G1 Z-.5 F50;
G13 D1 I0.225 K1.25 Q0.25 F4.07;
G0 Z1.0 M9;
G40; |
 |
The line of program code that mills
the circle is:
G13 D1 I0.225 K1.25 Q0.25 F4.07;
G13 = the counter clockwise spiral bore command
D1 = enable tool radius compensation
I0.225 = start position diameter
K1.25 = ending diameter (part size)
Q0.25 = width of cut per spiral
| Programming
considerations |
|
This example programs to the center of the end mill. This
means that the program values need to allow for the radius of
the cutter. We can then start with the tool cutter radius
value with a zero setting in the offset file. |
 |
To mill
this counterbore we are using a 0.750 diameter 4-flute end
mill. The part has a pre-drilled 1.250 diameter hole. The G13
code programs a spiral interpolation to create a 3.250 diameter
hole. |
Our cutter SFPM is 200 with a 0.001 chip load.
The
I value is calculated based on a diameter of 1.200. This is the
pre-drilled hole diameter of 1.250 less a 0.050 clearance move
(1.250 – 0.050 = 1.200). We will feed the endmill down in the
Z axis at the 1.200 diameter position to clear the pre-drilled
hole.
Approach diameter = 1.200"
I value = (part diameter – cutter diameter) ÷ 2
I value = (1.200 – 0.750) ÷ 2 = I0.225
Ending diameter = 3.250 (bore size)
K value = (part diameter – cutter diameter) ÷ 2
K value = (3.250 – 0.750) ÷ 2 = K1.25
The Q value should not exceed 2/3 of
the cutter diameter in general. The actual width of the spiral
depends on the cutting conditions.
Note that the G12/G13 commands enable cutter compensation
without the need of the G41/G42 codes. You still must use the
G40 command to cancel the cutter comp.
|
|
| The
end mill spirals to open the drilled hole into the
required counter bore. |
|
|
Advantages
The main advantage is the ease of
programming. With other circle
milling programming methods, the coding is more complex. This is a
great method to machine chuck jaws for gripping round parts.
With G12/G13 you can mill the same bore in a
number of spots with the same program codes. Just change the hole’s
absolute start point and away you go!
This method has been around for a long time,
give it a try. It can be a real handy programming method for many
uses. |
