G72 Bolt Holes Along an Angle (Group 00)

Next Generation Control Mill Operator's Manual

The Online Interactive Operator's Manual is currently available in English only.

A PDF version of the Operator's Manual is available for download in multiple languages. Click the link below to view the Operator's Manual in your language. Click "Continue" to view the online version in English.

I - Distance between holes
*J - Angle of line (degrees CCW from horizontal)
L - Number of holes

*indicates optional

This non-modal G code drills L number of holes in a straight line at the specified angle. It operates similarly to G70. For a G72 to work correctly, a canned cycle must be active so that at each position, a drill or tap function is performed.

G70, G71, and G72 Bolt Holes: [I] Radius of bolt circle (G70, G71), or distance between holes (G72), [J] Starting angle from the 3 o’clock position, [K] Angular spacing between holes, [L] Number of holes.

Rules for Bolt Pattern Canned Cycles

1. Place the tool at the center of the bolt pattern (for G70 or G71), or at the starting hole location (for G72), before the canned cycle execution.
2. The J code is the angular starting position and is always 0 to 360 degrees counterclockwise from the three o’clock position.
3. For G70 and G71 cycles, put an L0 on the initial canned cycle line to skip drilling at the center of the hole pattern. You can also turn off Setting 28 to prevent a hole from being drilled at the initial X/Y position. Refer to page 28 - Can Cycle Act w/o X/Y for more information on Setting 28.
4. For G70 and G71 cycles, put an L0 on the initial canned cycle line to skip drilling at the center of the hole pattern. You can also turn off Setting 28 to prevent a hole from being drilled at the initial X/Y position. Refer to Setting 28 - Can Cycle Act w/o X/Y for more information on Setting 28.
5. For G70 and G71 cycles, put an L0 on the initial canned cycle line to skip drilling at the center of the hole pattern. You can also turn off Setting 28 to prevent a hole from being drilled at the initial X/Y position. Refer to page 28 - Can Cycle Act w/o X/Y for more information on Setting 28.
note: L0 is the preferred method.
*D - Depth of cut for each pass of stock removal, positive
*F - Feedrate in inches (mm) per minute (G98) or per revolution (G99) to use throughout G71 PQ block
*I - X-axis size and direction of G72 rough pass allowance, radius
*K - Z-axis size and direction of G72 rough pass allowance
P - Starting Block number of path to rough
Q - Ending Block number of path to rough
*S - Spindle speed to use throughout G72 PQ block
*T - Tool and offset to use throughout G72 PQ block
*U - X-axis size and direction of G72 finish allowance, diameter
*W - Z-axis size and direction of G72 finish allowance

*indicates optional

G18 Z-X plane must be active.

G72 Basic G Code Example: [P] Starting block, [1] Start position, [Q] Ending block.

% O60721 (G72 END FACE STOCK REMOVAL EX 1) ; (G54 X0 is at the center of rotation) ; (Z0 is on the face of the part) ; (T1 is an end face cutting tool) ; (BEGIN PREPARATION BLOCKS) ; T101 (Select tool and offset 1) ; G00 G18 G20 G40 G80 G99 (Safe startup) ; G50 S1000 (Limit spindle to 1000 RPM) ; G97 S500 M03 (CSS, spindle on CW) ; G00 G54 X6. Z0.1 (Rapid to clear position) ; M08 (Coolant on) ; G96 S200 (CSS on) ; (BEGIN CUTTING BLOCKS) ; G72 P1 Q2 D0.075 U0.01 W0.005 F0.012 (Begin G72) ; N1 G00 Z-0.65 (P1 - Begin toolpath); G01 X3. F0.006 (1st position); Z-0.3633 (Face Stock Removal); X1.7544 Z0. (Face Stock Removal) ; X-0.0624 ; N2 G00 Z0.02 (Q2 - End toolpath); G70 P1 Q2 (Finish Pass) ; (BEGIN COMPLETION BLOCKS) ; G97 S500 (CSS off) ; G00 G53 X0 M09 (X home, coolant off) ; G53 Z0 M05 (Z home, spindle off) ; M30 (End program) ; %

G72 Tool Path: [P] Starting block, [1] Start position, [Q] Ending block.

% O60722(G72 END FACE STOCK REMOVAL EX 2) ; (G54 X0 is at the center of rotation) ; (Z0 is on the face of the part) ; (T1 is an end face cutting tool) ; (BEGIN PREPARATION BLOCKS) ; T101 (Select tool and offset 1) ; G00 G18 G20 G40 G80 G99 (Safe startup) ; G50 S1000 (Limit spindle to 1000 RPM) ; G97 S500 M03 (CSS, spindle on CW) ; G00 G54 X4.05 Z0.2 (Rapid to 1st position) ; M08 (Coolant on) ; G96 S200 (CSS on) ; (BEGIN CUTTING BLOCKS) ; G72 P1 Q2 U0.03 W0.03 D0.2 F0.01 (Begin G72); N1 G00 Z-1.(P1 - Begin toolpath) ; G01 X1.5 (Linear feed) ; X1. Z-0.75 (Linear feed) ; G01 Z0 (Linear feed) ; N2 X0(Q2 - End of toolpath) ; G70 P1 Q2 (Finishing cycle) ; (BEGIN COMPLETION BLOCKS) ; G97 S500 (CSS off) ; G00 G53 X0 M09 (X home, coolant off) ; G53 Z0 M05 (Z home, spindle off) ; M30 (End program) ; %

This canned cycle removes material on a part given the finished part shape. It is similar to G71 but removes material along the face of a part. Define the shape of a part by programming the finished tool path and then use the G72 PQ block. Any F,S or T commands on the G72 line or in effect at the time of the G72 is used throughout the G72 roughing cycle. Usually a G70 call to the same PQ block definition is used to finish the shape.

Two types of machining paths are addressed with a G72 command.

• The first type of path (Type 1) is when the Z Axis of the programmed path does not change direction. The second type of path (Type 2) allows the Z Axis to change direction. For both the first type and the second type of programmed path the X Axis cannot change direction. If Setting 33 is set to FANUC, Type 1 is selected by having only an X-axis motion in the block specified by P in the G72 call.

• When both an X-axis and Z-axis motion are in the P block then Type 2 roughing is assumed. If Setting 33 is set to YASNAC, Type 2 is specified by including R1 on the G72 command block (Refer to Type 2 details).

G72 End Face Stock Removal Cycle: [P] Starting block, [1] X-Axis clearance plane, [2] G00 block in P, [3] Programmed path, [4] Roughing allowance, [5] Finishing allowance.

The G72 consists of a roughing phase and a finishing phase. The roughing and finishing phase are handled differently for Type 1 and Type 2. Generally the roughing phase consists of repeated passes along the X-axis at the specified feed rate. The finishing phase consists of a pass along the programmed tool path to remove excess material left by the roughing phase while leaving material for a G70 finishing cycle. The final motion in either type is a return to the starting position S.

In the previous figure the start position S is the position of the tool at the time of the G72 call. The X clearance plane is derived from the X-axis start position and the sum of U and optional I finish allowances.

Any one of the four quadrants of the X-Z plane can be cut by specifying address codes I, K, U, and W properly. The following figure indicates the proper signs for these address codes to obtain the desired performance in the associated quadrants.