CNC Macro Programming for Custom Deep Hole Cycles

Standard canned cycles (G73, G83) handle basic deep hole drilling needs, but they have fixed behavior: constant peck depth, constant feed rate, and no conditional logic. For advanced deep hole drilling — where parameters should change as the hole gets deeper — custom macro programming provides the flexibility needed.

This guide covers Fanuc Custom Macro B, the most widely used macro language, with examples adaptable to other controls.

Why Custom Macros for Deep Hole Drilling?

Standard G83 Limitation	Custom Macro Solution
Fixed peck depth (Q)	Variable peck depth — decreasing at depth
Fixed feed rate	Variable feed — slower at entry and exit
No conditional logic	Monitor depth, adjust parameters in real time
No coolant control	M-code before each peck can turn coolant on/off
No first-peck adjustment	First peck deeper (or shallower) than subsequent pecks
No manual chip evacuation	Programmed dwell or spindle reverse at final depth

Fanuc Custom Macro B Basics

Variables

Variable Type	Range	Persistence
Local	#1–#33	Cleared on program end
Common	#100–#199	Cleared on power off
Common	#500–#999	Retained on power off
System	#1000+	Machine parameters, position, status

Macro Call with Arguments

; Call macro O9001 with arguments
G65 P9001 X25.0 Y0 Z-40.0 R2.0 Q4.0 F150

Arguments are passed to local variables:

Letter	Variable	Meaning
X	#24	X position
Y	#25	Y position
Z	#26	Z depth
R	#18	R-plane
Q	#17	Peck depth
F	#9	Feed rate

Example 1: Variable Peck Depth Macro

This macro decreases peck depth as the hole gets deeper, providing more frequent chip evacuation at depth.

% (MACRO: VARIABLE PECK DRILL)
O9001 (VARIABLE PECK DRILL)
#30=#24 (X POSITION)
#31=#25 (Y POSITION)
#32=#26 (Z DEPTH - FINAL)
#33=#18 (R PLANE)
#34=#17 (INITIAL PECK DEPTH)
#35=#9  (FEED RATE)

#1=#33   (CURRENT Z POSITION - START AT R PLANE)
#2=#34   (CURRENT PECK DEPTH - START AT INITIAL)

WHILE [#1 GT #32] DO1  (LOOP UNTIL REACH FINAL DEPTH)
  IF [#1 - #2 LT #32] THEN #2=#1 - #32 (LAST PECK - REDUCED)

  G01 Z[#1 - #2] F#35  (FEED TO PECK DEPTH)
  G00 Z[#33]            (RETRACT TO R PLANE)
  G00 Z[#1 - 0.5]       (RAPID BACK TO LAST DEPTH - MINUS CLEARANCE)

  #1=#1 - #2            (UPDATE CURRENT DEPTH)
  #2=#2 * 0.9           (REDUCE NEXT PECK BY 10%)
  IF [#2 LT 1.0] THEN #2=1.0 (MINIMUM PECK 1.0 MM)
END1

G00 Z#33 (FINAL RETRACT)
M99

Calling the macro:

G65 P9001 X25.0 Y0 Z-40.0 R2.0 Q6.0 F150

Behavior: First peck 6 mm, second 5.4 mm, third 4.9 mm, down to minimum 1.0 mm.

Example 2: Entry Feed Reduction Macro

This macro uses a reduced feed for the first peck, then increases to the production feed rate.

O9002 (ENTRY FEED REDUCTION DRILL)
#24=#24 (X)
#25=#25 (Y)
#26=#26 (Z)
#18=#18 (R)
#17=#17 (Q)
#9=#9   (PRODUCTION FEED)
#7=#7   (ENTRY FEED - PASSED AS E ARGUMENT)

G00 X#24 Y#25  (MOVE TO POSITION)
G00 Z#18        (RAPID TO R PLANE)

; FIRST PECK - REDUCED FEED
G01 Z[#18 - #17] F#7
G00 Z#18
G00 Z[#18 - [#17 - 0.5]]

; REMAINING PECKS - FULL FEED
#1=#18 - #17
WHILE [#1 GT #26] DO1
  IF [#1 - #17 LT #26] THEN #17=#1 - #26
  G01 Z[#1 - #17] F#9
  G00 Z#18
  G00 Z[#1 - 0.5]
  #1=#1 - #17
END1

G00 Z#18
M99

Calling the macro:

G65 P9002 X25.0 Y0 Z-40.0 R2.0 Q4.0 E80 F150

Entry feed = 80 mm/min, production feed = 150 mm/min.

Example 3: Coolant-Controlled Deep Hole Cycle

For machines without through-spindle coolant, turning coolant on and off between pecks can improve chip evacuation.

O9003 (COOLANT CONTROL DRILL)
G00 X#24 Y#25
G00 Z#18

#1=#18
WHILE [#1 GT #26] DO1
  IF [#1 - #17 LT #26] THEN #17=#1 - #26

  M08           (COOLANT ON BEFORE CUT)
  G01 Z[#1 - #17] F#9
  G04 P200      (DWELL 0.2 SEC)
  M09           (COOLANT OFF FOR RETRACT)
  G00 Z#18      (CLEAR RETRACT)
  M08           (COOLANT ON BEFORE NEXT PECK)
  G00 Z[#1 - 0.5]

  #1=#1 - #17
END1

M09
M99

Example 4: Position-Specific Parameter Adjustment

For drilling multiple holes at different depths, this macro adjusts feed rate based on hole depth.

O9004 (POSITION-SPECIFIC DRILL)
; X=#24, Y=#25, Z=#26 (FINAL DEPTH)
; FEED = 100 + ABS(Z)/10 (DEEPER = FASTER FEED)

#9 = 100 + [ABS[#26] / 10]

G83 X#24 Y#25 Z#26 R#18 Q#17 F#9
M99

Mapping Custom Cycles to G-Codes

Custom macros can be mapped to user-defined G-codes for easier calling:

System Variable	Maps To
#6050	Macro O9011 → G-code (e.g., G123)
#6051	Macro O9012
#6052–#6059	Macros O9013–O9020

Setup:

; Set parameter #6050 to 123
; Now G123 calls macro O9011
G123 X25.0 Y0 Z-40.0 R2.0 Q4.0 F150

Siemens Sinumerik Custom Cycles

Siemens controls use a different approach — high-level language (SCL) or SINUMERIK Operate cycles:

; Sinumerik custom cycle example
PROC CYCLE84 (REAL RTP, REAL RFP, REAL SDIS, REAL DP, REAL DPR)
  ; Custom deep hole cycle
  G0 G90 X0 Y0
  G1 Z=RFP+SDIS F500
  ; ... custom logic
  M17

Macro Programming Best Practices

Practice	Why
Document variable usage	Macros are hard to debug without documentation
Use modal-safe programming	Save and restore G90/G91, G98/G99, and other modal states
Include clearance moves	Always retract at least 0.5 mm above the previous depth
Test on a simulation first	Macro bugs can cause rapid moves into the workpiece
Use WHILE loops, not GOTO	WHILE loops are safer and more readable
Set minimum peck depth	Prevent infinite loops with decreasing peck macros

Summary

Custom macro programming extends the deep hole drilling capability of standard CNC machines far beyond what G73 and G83 offer. Variable peck depth (decreasing at depth), entry feed reduction, coolant control, and position-specific parameter adjustment are all achievable with Fanuc Custom Macro B or similar macro languages on other controls. For production deep hole drilling beyond 15:1 depth ratio, custom macros combined with through-spindle coolant provide a cost-effective alternative to dedicated deep hole drilling equipment.

For G83/G73 fundamentals, see CNC deep hole drilling G-code guide. For control-specific cycles, see CNC drilling cycles by control. For a complete overview, visit the CNC deep hole drilling guide.