Unique G-Codes pptx

HAAS UNIQUE G-CODES

G12/13 - CIRCULAR POCKET MILLING
G12/13 - CIRCULAR POCKET MILLING

G51 - SCALING
G51 - SCALING

G53 - NON-MODAL MACHINE
G53 - NON-MODAL MACHINE
COORDINATE SYSTEM
COORDINATE SYSTEM

G68 - ROTATION
G68 - ROTATION

G101 - MIRROR IMAGE
G101 - MIRROR IMAGE

G150 GENERAL PURPOSE POCKET
G150 GENERAL PURPOSE POCKET
MILLING
MILLING
UNIQUE MILL G-CODES
OVERVIEW
•
Description of Codes
•
Code Format
•
Effects of Settings

•
Unique Features
•
Examples
G12/G13-CIRCULAR
POCKET MILLING
•
Used for milling circular pockets
•
G12 [D ] [F… ] [I…] [K… ] [L…]
[Q…] [Z…] (Clockwise move)
•
G13 is used for counter clockwise
moves

D - Tool radius offset selection

F - Feedrate

I - Radius of first circle(or finished circle
if no K)

K - Radius of finished circle (optional)

L - Loop count for deeper pockets (used
with a G91)

Q - Incremental radius step (required
with K)


Z - Depth of cut (or increment with L)
This is an standard feature
G12/G13-CIRCULAR
POCKET MILLING (cont)
•
G12 and G13 are Non-modal
•
Cutter Compensation is included
in this routine
•
Use D00 to ignore tool offset
•
Use I without K and Q for small
pockets or holes
•
When using K and Q, only K
should be the radius of the
desired finished pocket
•
Position cutter in a previous
block or add an X and Y to the
G12/G13 line
G12 Example using I
(Finished Radius)
O0010 ;
T1 M06 ;
G90 G54 G00 X1.0 Y1.0 ;
S1500 M03 ;
G43 Z0.1 H1 M08;
G12 Z-0.5 I0.4 D01 F15. ;

G12 Z-0.5 I0.4 D01 F15. ;
G00 Z0.1 M09 ;
G28 G91 Y0 Z0 ;
M30 ;
Only one pass is required for
this example, so there is only
an I value (circle radius) in the
G12 line. G12 will use
conventional rather than
climb milling
We want to mill a 0.8” diameter
0.5” deep pocket using a 0.5”
endmill. The picture shows the
tool path for the code given.
G13 Example
using I, K, Q
O0010 ;
T1 M06 ;
G90 G54 G00 X1.0 Y1.0 ;
S1500 M03 ;
G43 Z0.1 H1 M08;
G12
G12
G91
G91
Z-0.5 I0.3
Z-0.5 I0.3
K1.5 Q0.3
K1.5 Q0.3

D01 F15.
D01 F15.
L3
L3
;
;
G90 ;
G00 Z0.1 M09 ;
G28 G91 Y0 Z0 ;
M30 ;
This example requires more
passes in both the radius and
depth so K, Q and L (and a
G91) are used in addition to I.
We want to mill a 3.0” diameter
1.5” deep pocket using a 0.5”
endmill.
As seen in the picture, the first pass
is the I value (0.3”). Additional passes
of Q increments (also 0.3”) are made
until the full radius (K1.5) is cut. Then
the tool will move down in Z another
0.5” and repeat the process. The G13
cycle will repeat three times (L3) to
produce a depth of 1.5”
G51-SCALING
•
Used to proportionally increase or
decrease X, Y, Z, I, J, K, or R

values in subsequent lines of
code
•
G51 [X…] [Y…] [Z…] [P…]

X - Optional X-axis center of scaling

Y - Optional Y-axis center of scaling

Z - Optional Z-axis center of scaling

P - Optional scaling factor, 3 place
decimal from 0.001 to 8383.000
•
With G51, you can easily create
different size parts by just
changing the P value.
•
G50 - Cancel Scaling
This is an optional feature along with G68 - Rotation.
G51-SCALING
(cont)
•
Setting 71- If P is not used, Setting 71
is the default scaling factor.

G51 X1. 5 Y1.0 (Scaling center is at X1.5,
Y1.0 and the scale factor is determined by
Setting 71)
•

If X, Y, or Z are not used, the current
work coordinate is used as the
scaling center

G00 X1.0 Y2.0

G51 P2. (Scaling center is at X1.0, Y2.0
with a scale factor of 2.)
The factory default for setting 71 is 1.0,
meaning no scaling would take place.
G51-SCALING
(Example)
O0010 ;
T1 M06 ;
G54 G90 G00 X0 Y0 ;
G43 Z0.1 H1 ;
S500 M03 ;
G51 P2.
G51 P2.
;
; (Scale factor of 2.)


M97 P10 ;
G28 G91 Y0 Z0 ;
M30 ;
N10 G00 X1. Y1. ;
G01 Z-0.5 F15. ;
X2. F20. ;
Y2. ;

G03 X1. R0.5 ;
G01 Y1. ;
G00 Z0.1 ;
M99 ;
(Original
geometry)
Take geometry shown by dashed line and
double the size. Use the original work
coordinate origin as the scaling center.
= Work coordinate origin
= Center of scaling
Z values will also be doubled, so
depth of pocket will be -1.0.
G51-SCALING
(Example 2)
O0010 ;
T1 M06 ;
G54 G90 G00 X0 Y0 ;
G43 Z0.1 H1 ;
S500 M03 ;
G51 X1.5 Y1.5 P2
G51 X1.5 Y1.5 P2
.;
.;
M97 P10 ;
G28 G91 Y0 Z0 ;
M30 ;
N10 G00 X1. Y1. ;
G01 Z-0.5 F15. ;
X2. F20. ;

Y2. ; G03 X1. R0.5 ;
G01 Y1. ;
G00 Z0.1 ;
M99 ;
(Original
geometry)
Take geometry shown by dashed line and
double the size. Use a different work
coordinate as the scaling center.
= Work coordinate origin
= Center of scaling
(Scaling center
X1.5 Y1.5)
G51-SCALING (Example 3)
O0010 ;
T1 M06 ;
G54 G90 G00 X0 Y0 ;
G43 Z0.1 H1 ;
S2500 M03 ;
G51 P1.5
G51 P1.5
;
; (Scale Factor of 1.5)
M97 P10 ;
G28 G91 Y0 Z0 ;
M30 ;
N10 G00 X-0.125. Y-0.2. ;
G01 Z-0.5 F50. ;
Y3.125. F20. ;
G02 X0.25Y3.375 R0.375 ;

G01 X1.6562 ;
G02 x2. Y3.0313 R0.3437 ;
G01 Y2.125 ;
G03 X2.375 Y1.75 R0.375 ;
G01 X3.5 ;
G02 4. Y1.25 R0.5 ;
G01 Y0.4375 ;
G02 X3.4375 Y-0.125 R0.5625 ;
G01 X-0.2 ;
G00 Z0.1 M09 ;
M99 ;
(Original
geometry)
The smaller area is the original geometry.
You can make the part 1.5 times larger
with a G51 P1.5 like shown at right.
= Work coordinate origin
= Center of scaling
G53-NON-MODAL
COORDINATE SYSTEM
•
Cancels existing work coordinate
system
•
Can be used to return spindle or
table to machine zero

G53 Y0.

Moves table to machine zero in Y

•
Must be used with a G49 if you have
a Z value (G49 cancels tool offset)

G53 G49 Z0.

Returns spindle to machine zero
•
An alternative to G28 G91 Z0;

With G28 you must remember to add a
G90 afterwards
•
With G53 you stay in G90 mode
This is a standard
feature.
G68-ROTATION
•
Used to rotate subsequent X, Y, Z, I,
J, or K values by a specified angle
using a center of rotation
•
[G17] [G18] [G19] G68 [a] [b] [R]

G17, G18, G19 - Plane of Rotation

a - Center of rotation for the first axis

b - Center of rotation for the second
axis


R - Angle of rotation in degrees, from
-360.000 to -360.000, 3-place decimal
•
G69 - Cancels G68-Rotation
This is an optional feature along with G51 - Scaling.
G68-ROTATION
(cont)
•
Setting 72 - If R is not included in
the G68 line, Setting 72 is the
default angle of rotation
•
Setting 73 - Must be on to have the
rotational value incrementally
change in G91 mode
•
Can be combined with Scaling -
Scaling should be activated first
•
Cutter Comp should be turned on
after G51 or G68 commands and
turned off before G50 and G69.
The factory default of Setting 72 is 0.0.
G68 - ROTATION
(Example)
O0010 ;
T1 M06 ;
G54 G90 G00 X0 Y0 ;
G43 Z0.1 H1 ;

S500 M03 ;
M97 P10 L8;
G69 M09 ;
G28 G91 Y0 Z0 ;
M30 ;
N10 G91 G68 X0 Y0 R45.
N10 G91 G68 X0 Y0 R45. ;
G90 ;
G00 X1. Y1. Z0.1 ;
G01 Z-0.5 F15. M08 ;
X2. F20. ;
Y2. ;
G03 X1. R0.5 ;
G01 Y1. ;
G00 Z0.1 ;
M99 ;
We will take one of the arched windows
and rotate it around the origin in 45
degree increments.
= Work coordinate origin
= Center of scaling
(Window
geometry)
By altering the “L” and “R” in the underlined blocks you can vary
the number of windows cut.
(Rotate 45°)
(Pocket routine is
done 8 times.)
O0010 ;
T1 M06 ;

G54 G90 G00 X0 Y0 ;
G43 Z0.1 H1 ;
S500 M03 ;
M97 P10 L6;
G69 M09 ;
G28 G91 Y0 Z0 ;
M30 ;
N10 G91 G68 X0 Y0 R60.
N10 G91 G68 X0 Y0 R60. ;
G90 ;
G00 X-0.4911 Y2.9062 ;
G01 Z-0.5 F15. M08 ;
G02 X0.4911 Y2.9062 I0.4911 J0.0938;
G01 X0.1228 Y0.9774 ;
G02 X-0.1228 Y0.9766 I-0.1228 J0.0234;
G01 X-0.4911 Y2.9062
G00 Z0.1 ;
M99 ;
We will take a pocket that is
uniform around the X-axis, and
rotate it around the origin in 60
degree increments.
= Work coordinate origin
= Center of scaling
(Pocket
geometry)
Note that in this and the last example we included an X and Y in
the G68 line to define the center of rotation.
(Rotate 60°)
G68 - ROTATION

(Example 2)
G101-MIRROR IMAGE
•
Used to produce a mirror image of a
sequence of codes around an X, Y,
Z, A or B axis
•
G101 [X] [Y] [Z] [A] [B]

At least one axis must be specified

Any value given will be ignored

G100 cancels mirror image
You can mirror image more than one axis at a time.
This is an standard control feature.
•
Setting 45 - Mirror image X-axis
•
Setting 46 - Mirror image Y- axis
•
Setting 47 - Mirror image Z-axis
•
Setting 48 - Mirror image A-axis
•
Setting 80 - Mirror image B-axis
•
These settings activate mirror imaging
without using G101
•

If only one axis is mirrored, climb
milling will be changed to
conventional milling (i.e. direction of
travel will be reversed). Cutter
compensation is also reversed.
When you use these settings, mirror imaging will be
active until you manually turn the settings off.
G101-MIRROR IMAGE
(cont)
G101-MIRROR IMAGE
(Example)
In this example, we will mirror
the Pocket on the right in the X-
axis, producing a similar pocket
on the left.
O0010 ;
T1 M06 ;
G54 G90 G00 X0 Y0 ;
G43 Z0.1 H1 ;
S500 M03 ;
M97 P20 ;
N10 G101 X0
N10 G101 X0 ;
M97 P20 ;
G100
G100 ;
G00 Z0.1 ;
M09 ;
G28 G91 Y0 Z0 ;
M30 ;

N20 G00 X-0.4653 Y0.052 ;
G01 Z-0.5 F15. M08 ;
G01 X-1.2153 Y0.552 ;
G03 X-1.3059 Y0.528 R.0625 ;
G01 X-1.5559 Y0.028 ;
G03 X-1.5559 Y-0.028 R.0625 ;
G01 X-1.3059 Y-0.528 ;
G03 X-1.2153 Y-0.552 R.0625 ;
G01 X-0.4653 Y-0.052 ;
G03 X-0.4653 Y0.052 R.0625 ;
M99 ;
Because the pocket is symmetrical around the
X-axis, we could add a Y0 in line N10 and not
change the part. This would allow us to Climb
Mill on the second pocket as well as the first.
(Pocket
geometry)
G101-MIRROR IMAGE
(Example 2)
O0010 ;
T1 M06 ;
G54 G90 G00 X0 Y0 ;
G43 Z0.1 H1 ;
S500 M03 ;
M97 P10 ;
N10 G101 Y0
N10 G101 Y0 ; (Mirror in Y-axis)


M97 P20 ;

G28 G91 Y0 Z0 ;
M30 ;
N20 G00 X2. Y2. ;
G01 Z-0.5 F15. ;
X4. F20. ;
Y4. ;
G03 X2. R1. ;
G01 Y2. ;
G00 Z0.1 ;
M99 ;
(Original
geometry)
In this example, we will mirror the pocket on
top, in the Y-axis, producing a similar
pocket on the bottom.
In this example, Climb Milling on the first pocket is changed
to Conventional on the second pocket.
G101-MIRROR IMAGE
(Example 3)
O0010 ;
T1 M06 ;
G54 G90 G00 X0 Y0 ;
G43 Z0.1 H1 ;
S500 M03 ;
M97 P10 ;
N10 G101 Y0
N10 G101 Y0
X0
X0; (Mirror in X-
M97 P20 ; and Y- axes)

G28 G91 Y0 Z0 ;
M30 ;
N20 G00 X2. Y2. ;
G01 Z-0.5 F15. ;
X4. F20. ;
Y4. ;
G03 X2. R1. ;
G01 Y2. ;
G00 Z0.1 ;
M99 ;
If we add an X0 to line N10, it will
produce results shown above.
Climb Milling will also take place
on the second pocket.
G150-POCKET MILLING
•
Used to mill a pocket by defining only the
outside shape of the pocket
•
G150 G41* P… F… D… I… J… K… Q… R…
X… Y… Z… [L…] [S…]

P - Number of Sub-program defining pocket(required)

F - Feedrate

D - Tool diameter offset selection

I - X-axis cut increment (I or J is required)


J - Y-axis cut increment

K - Finish cut allowance

Q - Incremental Z-axis cut depth per pass (>0) (reqiuired)

R - R plane position (required)

X & Y - Position of starting hole

Z - Final depth of pocket

L - Optional repetition count for additional pockets

S - Optional spindle speed
* G42, Cutter Comp Right, is also permissible
This is an standard control feature.
G150-POCKET
MILLING (cont)
•
You should first drill a hole at the X,Y entry
location.
•
The Pocket definition must be in a Sub-
program, not a subroutine.
•
The Sub-program must have less than 40
strokes.

Codes other than G, I, R, X and Y in the Sub-

program are ignored

The first move in the Sub-program should be from
the clearing hole to a point on the pocket edge

The last move in the Sub-program should be to
that same starting point on the pocket edge

You can use either G91 (Incremental) or G90
(Absolute) moves in the Sub-program
G150-POCKET
MILLING (cont)
•
There is no finishing pass in the Z depth.
•
Q is a positive value for the amount of
incremental step down in Z for deeper pockets.
•
You cannot use both I and J.
•
If you use L for additional pockets, you must have
a G91 and incremental positioning in the G150
line
–
You will also need to drill all your clearing holes prior to
the G150 line
•
The finishing pass, K, is taken at the full depth (Z)
of the pocket.
•

It is also possible to program an island within a
pocket. (See the Operators Manual for an example of
this.)
•
You can not use a G68 with G150