Service Home G156 Broaching Canned Cycle (Group 09)

G156 Broaching Canned Cycle (Group 09)

G156 Broaching Canned Cycle (Group 09)

Z - Z-axis absolute location total pecking depth.
W - Z-axis incremental distance to total pecking depth.
* Y - Y-axis absolute location of furthest slice cycle (diameter).
* V - Y-axis incremental distance to furthest slice (diameter).
X - X-axis absolute location of furthest slice cycle (diameter)
* U - X-axis incremental distance to furthest slice (diameter).
* I - X-axis size of increment between slice cycles.
* K - Z-axis size of increment between pecks in a cycle.
* F - Feed rate per minute.
* C - C-axis position.
* D - Tool clearance when returning to starting plane.
*indicates optional

NOTE: The machine must have software version 100.20.000.1000 or higher to use this G-code.
G156 Broaching Canned Cycle: [1] Rapid, [2] Feed, [3] Programmed Path, [C] Clearance Point, [K] Peck ,[22] Peck retraction (Setting 22).


Broaching operations canned cycle can be done using a single tool path (with adjustable programmable Pecks) when using a special broaching shape tool.


Spindle orient command M19P/R code which used to position the spindle before broaching must be used first before executing G156 broaching canned cycle.

NOTE: M19, P, or R should not be on the same line as G156. M19, P, or R value should not be negative. See
M19
for more information.
When K is added to a G156 block, then pecking will be performed at each interval specified by K.The D code can be used for grooving and turning to provide material clearance when returning to starting plane S.The D code command is used to provide a tool clearance shift, in the X-axis before returning in the Z-axis to the "C" clearance point.When an X/U, or Y/V code is added to a G156 block and the current (i.e. actual) X/U, Y/V axes machine position not at the position defined by G156X/U, Y/V, then a minimum of two pecking canned cycles will occur, one at the current (actual) location of the machine X/U, Y/V axes, and another one at the X/U, Y/V location set by G156.The I code is the incremental distance (slices cycle) between the start position S toward the target X/U, Y/V Axes positions (i.e. the thickness of each slice).Adding an I will performs multiple, evenly spaced, slice cycles between the starting position S and X/U, Y/V Axes target position.When the distance between S and target X/U, Y/V is not evenly divisible by I, then the last interval is less than I.The spindles shall be positioned first (Main/Sup spindle) by either having the C-axis engaged (For Main spindle) or spindle to be oriented (Main/Sub) before staring the broach cycle.

NOTE: An alarm will be generated when using Cutting feed rate as unit/revolution with Lathe broaching canned cycle.
G112 (Cartesian to Polar coordinate transformation feature) is not allowed to be used in lathe broaching canned cycle and the control shall alarm out.The tool clearance shift direction (i.e. shift in + X or - X, ZX plane,) will be depend on the sign of the D value (Positive/Negative).When the D has a positive value, the tool moves in the positive direction of the X-axis.When the D has a negative value, the tool moves further in the negative direction of the X-axis.When D has a zero value or it not specified with the G156 lathe broaching canned cycle, then there shall be no tool clearance shift in the X-axis before returning in the Z-axis to the "C" clearance point.I.e. the tool returning in the Z-axis to the "C" clearance point will use the same peck path in the opposite direction.

NOTE: An alarm will be generated if any spindle commanded to turn (other than spindle orient/ c axis position) within broaching canned cycle, or the broaching canned cycle is starting the Pecks cycle and the spindle is still turning.
Cxx (position the C axis) could be use before or on the same line of G156 broaching canned cycle.Using the spindle brake before starting the broach cycle is recommended, but is not required.

NOTE: The broaching canned cycle is a modal, and it shall be repeated on each line within the canned cycle uses any broaching address code. Refer to examples below:

Lathe Broaching: Example 1

G-Code Program Sequence
%
O41322 ( BROACH SAMPLE PROGRAM);
G00 G54 G18 G40 G80 G97 G98;
G0 T101;
X1. Z.25;
C0.;
G156 X1.05 Y0. Z-1. I.0025 D0.01 F150.;
C45.;
C90.;
C135.;
C180.;
G80 G0 Z.25;
G28 X0. Z0.;
M30;
%
Safe Start Line
Tool 1 Offset 1
Rapid to Position
Position to C0.
Broach operations canned cycle start.
C-axis position.
End of Canned Cycle.

Lathe Broaching: Example 2

G-Code Program Sequence
%
G156 X-10. Y-2.0 Z-12.0 I0.5 K0.5 F10.;
X-5. Y-1.5 Z-10.0 I2.0 K2.0;
I1.0 K1.0;
C90.;
C45.0 X-5. Z-10.0 I2.0 K2.0;
G00 G80;
%
Lathe broaching operations canned cycle start.
Perform another broach with these new values at the current angle.
Perform another broach with these new values at the current angle.
Perform another broach at the new angle using the last specified address codes.
Rotate to new angle then broach using the new address codes.
End of canned cycle.

Lathe Broaching: Example 3

G-Code Program Sequence
%
G156 X-10. Z-12.0 I0.5 K0.5 F10. C45.; %
Position the C-axis first, then start the Lathe broaching operations canned cycle start (Spindle should not be turning).

Lathe Broaching: Example 4

G-Code Program Sequence
%
M19 P45 (or R45);
G156 X-10. Z-12.0 I0.5 K0.5 F10.;
M19 P90;
M19 P135;
C180.;
G00 G80;
%
Position the spindle (Using Spindle Orient).
Lathe broaching operations canned cycle start.
Repeat the canned cycle at this position.
Repeat the canned cycle at this position.
Position the C axis first (Using C-axis), then start the Lathe broaching operations canned cycle start.
End of canned cycle.
.

Lathe Broaching: Example 5

G-Code Program Sequence
%
C45.;
G156 X-10. Z-12.0 I0.5 K0.5 F10.;
C90.;
C135.;
M19 R180.;
M03 S2000 ;
M19 P200.;
G00 G80;
%
Position the spindle (Using C axis)
Lathe broaching operations canned cycle start
Repeat the canned cycle at this position
Repeat the canned cycle at this position
Using a different method (not C axis) to Position the spindle first, then start the Lathe broaching operations canned cycle start.
M03 S2000; Alarm: The spindle is running.
End of canned cycle
.

Lathe Broaching: Example 6

G-Code Program Sequence
%
M03 S2000 ;
G156 X-10. Z-12.0 I0.5 K0.5 F10.; %
Run the spindle
Alarm: The spindle is running.
.