Mazak EIA/ISO (G-Code) Programming — MAZATROL SmoothAi

Every Mazak machining center that ships with the EIA/ISO option runs two programming languages side by side: the conversational MAZATROL program the control is famous for, and standard EIA/ISO G-code — the same ISO dialect posted by any CAM system. This page covers the G-code side on the SmoothAi and SmoothG controls: how EIA programs are stored and selected, the G-code and M-code vocabulary, the drilling/boring canned cycles, and Mazak’s user-macro language (#-variables, arithmetic, IF/WHILE). Where Mazak’s dialect diverges from a Fanuc, those points are called out — do not assume a Fanuc habit carries over. See also the Mazak Control Guide for control operation.

How EIA/ISO Mode Works on a Mazak

On a MAZATROL control, a stored program is either a MAZATROL program (a conversational unit sequence) or an EIA/ISO program (line-oriented G-code). The control decides which interpreter to use from the program’s own content — there is no global “G-code mode” switch equivalent to Fanuc’s. You select the program to run from the program directory; a MAZATROL program opens in the conversational editor, an EIA program opens as a text-style G-code listing.

An EIA/ISO program is identified by a program number of the form O followed by an unsigned integer (the format spec permits up to eight digits, O8), or by a program name of up to 32 characters. The first significant line is typically a comment header in parentheses naming the part, followed by the setup block. A real Mazak header from a maker-supplied probing routine:

(O207409921 REN X DIAM)
(COPYRIGHT*2015-2017*RENISHAW*PLC.*ALL*RIGHTS*RESERVED)
M98P207409923          ; call a subprogram by O-number
#1=#5041               ; read present workpiece X into a local variable
...
M99                    ; return to caller (subprogram) / rewind (main)

EIA and MAZATROL programs coexist and can call each other. An EIA program calls a MAZATROL program the same way it calls any subprogram; the reverse is also supported. One rule the manual is emphatic about: when a MAZATROL program is called from an EIA/ISO program, the MAZATROL END unit must have CONTI. = 1 so control returns cleanly to the EIA main program — never put an M99 in the MAZATROL program to force the return.

Block and word rules that bite when hand-editing: a “word” with an address but no number (e.g. G28XY) is, by default (parameter F36 bit 3 = 0), treated as G28X0.Y0.; set that bit to 1 and the same block throws alarm 807 ILLEGAL FORMAT. Coordinate values without a decimal point are interpreted in the least input increment (0.0001 mm / 0.00001 in) — so X10 is 0.001 mm, not 10 mm. Always program a decimal point on dimensional data. G20/G21 (inch/metric) affect program data only; tool and offset data are not converted, so set those in the correct unit beforehand.

G-Code Reference

The following is the everyday subset of the SmoothAi EIA/ISO G-code list, grouped by function. The Group column is the modal group (codes in the same non-zero group are mutually exclusive and modal; group 00 codes are one-shot). Codes marked (option) are only present if the machine builder configured them. This is a working subset — the full list runs to well over a hundred codes including five-axis, turning, inclined-plane, and gear-cutting functions.

Drilling & Boring Canned Cycles

All hole-machining fixed cycles are modal group 09 and are canceled by G80 (or by any group-01 motion code such as G00). Return level is set by G98 (initial point) / G99 (R point). The typical format is G8x Xx Yy Zz Rr Ff [Qq] [Pp] [Ll] where Z is hole bottom, R is the rapid-approach (R) plane, Q is peck depth or shift, and P is a bottom dwell.

Watch the boring-cycle numbering. Mazak calls G75/G76/G78/G79/G86/G88/G89 “Boring 1–7,” and G74 is reverse tapping. On a Fanuc, G76 is fine boring, G74 is left-hand (counter) tapping, and G75/G78/G79 are not standard mill cycles. Do not assume a Fanuc canned-cycle number means the same thing here — check the cycle behavior in the manual before running a converted program.

M-Codes

The EIA/ISO manual defines a small set of NC-internal M-codes whose behavior is fixed by the control. Everything else (spindle, coolant, tool change, orientation) is a machine-configured miscellaneous function — the manual is explicit that whether such an M-code executes before, during, or after axis motion “depends on the machine specifications.” For those, consult the machine’s operation manual, not the EIA manual.

M00, M01, M02, M30, M998, and M999 all disable buffer pre-read, so a following block is not looked ahead. Real Mazak maker programs also use many machine-specific codes such as M111, M200, M203/M205, M648, and M787 — these are model-specific (probe arm, spindle selection on multi-tasking machines, sensor control) and their meaning must not be guessed; look them up for the specific machine.

User Macros — Variables

Mazak’s EIA/ISO user-macro language uses #-variables that will look familiar to anyone who knows Fanuc Custom Macro B, but the ranges and some system-variable numbers are Mazak-specific — verify them here rather than porting Fanuc numbers blind. A variable holds a value with an effective precision of 8 decimal digits; the null (undefined) variable is #0. A word whose value is an undefined variable (e.g. G#10 where #10 is null) is simply ignored.

Because Mazak stores tool data by tool-data index (not a fixed offset-register number as on Fanuc), read #3020 or #3022/#3023 to resolve the index for a given tool before indexing into the #40001+ arrays. This is a genuine Mazak/Fanuc difference: there is no direct equivalent of Fanuc’s #2001–#2400 fixed tool-offset block.

User Macros — Arithmetic & Flow Control

Assignment takes the form #i = <expression>, where the expression may mix constants, variables, functions, and operators. Up to five nested sets of brackets [ ] per expression (functions count toward that limit). Angles are in degrees.

Flow control:

Macros are called with G65 P_ L_ <arguments> (single call), G66/G66.1 (modal, canceled by G67), or as plain subprograms with M98. Under G65/G66, argument addresses map to local variables like Fanuc: A→#1 B→#2 C→#3 D→#7 E→#8 F→#9 H→#11 I→#4 J→#5 K→#6 M→#13 Q→#17 R→#18 S→#19 T→#20 U→#21 V→#22 W→#23 X→#24 Y→#25 Z→#26. Key difference from M98: G65 passes arguments and changes the local-variable level with call depth, and does not single-block-stop; M98 passes no arguments and keeps the same local-variable level.

A worked macro — a bolt-circle drilling routine using the argument mapping, trig, and a WHILE loop:

(O8001 BOLT CIRCLE)
G65 P8002 X0. Y0. R40. H8 Z-10. F150.   ; center X0 Y0, radius 40, 8 holes

(O8002 SUBMACRO)                        ; X#24 Y#25 R#18 H#11 Z#26 F#9
#30 = 360. / #11                        ; angle step = 360 / hole count
#31 = 0.                                ; running angle
#32 = 1                                 ; hole counter
G90 G81 R2. Z#26 F#9                     ; arm the spot/drill cycle (R plane 2 mm)
WHILE [#32 LE #11] DO1
#33 = #24 + #18 * COS[#31]             ; hole X = Xc + R*cos(angle)
#34 = #25 + #18 * SIN[#31]             ; hole Y = Yc + R*sin(angle)
X#33 Y#34                              ; drill at this position
#31 = #31 + #30
#32 = #32 + 1
END1
G80                                      ; cancel canned cycle
M99

Work Offsets & Tool Data in EIA Mode

EIA/ISO programs use the standard work coordinate systems G54–G59, the additional systems G54.1 P1–P300 (option), a local shift with G52, and the machine system directly with G53. Offset values are set on the WORK OFFSET / coordinate display, or written from a program with G10 (programmable data setting). Reference return is G28 via an intermediate point — almost every Mazak EIA program opens with an incremental reference return, e.g. G91 G28 Z0. then G28 X0. Y0., before the first tool change.

Tool geometry and wear live in the control’s TOOL DATA, indexed by tool number, and are applied through G43 H_ (length) and G41/G42 D_ (radius). Because the EIA offset addresses (H, D) point into the same shared tool table the MAZATROL side uses, a tool edited for a MAZATROL program changes what an EIA program sees under the same H/D number — the two languages are not sandboxed from each other on tool data. Note also that G20/G21 in a program do not re-scale already-stored tool or offset values.

Real-World Examples

A compact self-contained program — a Mazak spindle condition-check routine that steps through speeds with dwells (adapted from a maker-supplied program). It shows the reference-return preamble, tool call, and G04 dwell in seconds:

(CONDITION CHECK PROGRAM FOR 12000rpm)
T[#20]T00M06        ; tool change, pot number from variable #20
G91G28Z0.           ; incremental reference return, Z
G28X0.Y0.           ; reference return, X and Y
M200                ; (machine-specific: select/ready spindle)
M111                ; (machine-specific)
M03S1000            ; spindle CW, 1000 rpm
G04X60.             ; dwell 60 s
S5000
G04X60.
S9000
G04X60.
S12000
G04X120.            ; dwell 120 s at top speed
M05                 ; spindle stop
M30                 ; end + rewind

A macro/probing excerpt (adapted from a Renishaw X-diameter routine) showing G31 skip moves, reading captured positions from #5041/#5043, tolerance checks with IF[…]GOTO, and a sub-macro call with arguments:

#1=#5041                                ; store present workpiece X
#2=#5043-#116                           ; store present workpiece Z (minus clearance)
IF[#26EQ#0]GOTO2                        ; if Z-arg is null, skip the Z touch
#32=#7/2+#18                            ; half tool dia + overtravel
G31X[[#1*#108]-#32]F#119                ; probe toward -X at feed #119
IF[ABS[#5041-[#1-[#32/#108]]]GE#123]GOTO14   ; over tolerance -> error branch
N2
G65P207409926X[#1-[#7/2]]Q#17S#19      ; call reporting macro with args
G0Z#2                                    ; rapid clear in Z
M99

Note the real-program idiom IF[#4006 EQ 21] that these routines use to branch on metric (G21) vs. inch (G20) mode by reading the modal-G system variable — a clean example of using #4001–#4027 in practice.

Gotchas & Fanuc Differences

For conversational programming on the same control, see Mazak MAZATROL Programming; for control operation, screens, and setup, see the Mazak Control Guide.

References

• Yamazaki Mazak, Programming Manual (for Machining Centers) — EIA/ISO, MAZATROL SmoothAi, Manual No. H747PB1000E, 02.2020.
• Yamazaki Mazak, Programming Manual (for Machining Centers) — EIA/ISO, MAZATROL SmoothG, Manual No. H749PB1003E, 07.2022 (companion control).