Sinumerik ISO Mode (Running Fanuc-Style G-Code)
What ISO Dialect Mode Is
SINUMERIK 840D sl and 828D controls can run Fanuc-style G-code natively through the ISO dialect option — no translation required for most of the language. The control operates in one of two modes: Siemens mode (native language) or ISO dialect mode (Fanuc-style). You switch between them with two G-codes, each programmed alone in its own block:
| Command | Effect |
|---|---|
G290 | Siemens NC programming language active |
G291 | ISO dialect NC programming language active |
The active tool, tool offsets, and work offsets are not affected by the switchover. Which mode the control powers up and resets into is set by machine data: MD18800 $MN_MM_EXTERN_LANGUAGE activates the external language, and when ISO dialect is set as the default, the control reboots in ISO mode. Power-on defaults for the individual G groups (G90/G91, G20/G21, etc.) come from MD20154 $MC_EXTERN_GCODE_RESET_VALUES.
Ground rules the manual lays down:
| Rule | Consequence |
|---|---|
| No mixing dialects in one block | An NC block is either all ISO or all Siemens |
| No Siemens G-functions in ISO mode | Switch with G290 first if you need them |
| Siemens subroutines callable from ISO code | This is how the canned cycles actually run (Siemens shell cycles) |
| Max 9 axes in ISO mode | First three fixed as X, Y, Z; others from A, B, C, U, V, W |
What Works in ISO Mode
Appendix B of the manual lists the full ISO milling G-code table. The everyday Fanuc vocabulary is there. Codes marked optional depend on what the machine builder configured — check your machine documentation.
| Function group | G-codes supported | Notes |
|---|---|---|
| Motion | G00, G01, G02, G03, G33 | Plus helical G02/G03 and involute G02.2/G03.2 |
| Plane selection | G17, G18, G19 | Parallel-axis variants supported |
| Absolute / incremental | G90, G91 | |
| Inch / metric | G20, G21 | G-code system A/C variants (G70/G71) in the table |
| Feed modes | G93, G94, G95 | Inverse-time, per-minute, per-revolution |
| Cutter compensation | G40, G41, G42 | |
| Tool length compensation | G43, G44, G49 | Direction by sign of H offset, same as Fanuc |
| Canned cycles | G73, G74, G76, G80–G87, G89 | With G98/G99 return-plane control; multiple-start threads with G33 |
| Work offsets | G54–G59, G54.1 (G54 P1–48), G54 P0 | G54 P0 = external work offset; write offsets with G10 L2/L20 |
| Coordinate setting | G92, G92.1, G52, G53 | G92.1 resets G92/G52 shifts |
| Reference point | G27, G28, G30, G30.1 | |
| Scaling / mirroring | G50, G51, G50.1, G51.1 | Scaling is optional |
| Rotation | G68, G69 | 2D and 3D rotation; optional |
| Polar / special interpolation | G15, G16, G12.1, G13.1, G07.1 | G12.1 maps to Siemens TRANSMIT; G07.1 = cylindrical interpolation |
| Macros | G65, G66, G67 | See macro section — arguments land in Siemens variables |
| Measuring / skip | G31, G31 P1–P4, G10.6 | G10.6 = rapid lift via digital input |
| Subprograms / interrupts | M98, M99, M96, M97 | M96/M97 need MD10808 bit 0 enabled |
| Path control | G09, G61, G62, G63, G64 | Exact stop, corner override, tapping mode, continuous path |
| Other | G04, G10, G22, G23, G72.1, G72.2 | G72.1/G72.2 contour repetition (optional, not on all controls) |
What’s Different — the Gotchas
A Fanuc program will syntax-check its way through ISO mode, but several behaviors differ from a real Fanuc. These are the documented ones that bite.
| Area | On a real Fanuc | In Sinumerik ISO mode |
|---|---|---|
| No # macro variables | Macro B: #1–#33 locals, #100s, #500s, IF/GOTO/WHILE | Not part of the ISO milling dialect. G65/G66 arguments are stored in Siemens system variables $C_A–$C_Z, which can only be read in Siemens mode. Macro logic must be written in Siemens language (R-parameters, IF ... GOTOF) |
| Decimal-point handling | Set by parameter; typically X1000 = least-input-increment | MD10884 selects pocket-calculator notation (X1000 = 1000 mm) or standard notation (X1000 = 1 mm at IS-B, 0.1 mm at IS-C). Wrong setting scales every no-decimal value in the program |
| Subprogram numbers (M98) | M98 P51002 = O1002 × 5, programs live as O-numbers | M98 P21 searches part-program memory for the file 21.mpf; repeats via P30021 (count+number) or the L address. With 8-digit program numbers enabled (MD20734 bit 6), count-in-P is no longer allowed — the manual flags this as incompatible with the ISO original. Nesting: 16 levels (+2 reserved for interrupts) |
| Canned-cycle behavior data | Retract/clearance amounts from parameters (e.g., 5114) | Cycles run as Siemens shell cycles; safety clearance comes from GUD _ZSFR[0], G73 chip-break retract from _ZSFR[1], G76/G87 lift-off direction from _ZSFI[5]. Q is one modal value shared across G73/G76/G83 |
| Cycle modal data | Q and R stick once programmed | Program Q and R in a block that also has axis motion or the values are not stored modally; a G00–G03 in the same block deselects the cycle |
| Tool offset numbers (D/H) | D = radius offset register, H = length offset register | ISO D/H numbers map into the Siemens T/D tool memory through $TC_DPH[t,d], which someone must populate at setup. Length is always Z-assigned when $SC_TOOL_LENGTH_CONST = 17 |
| G31 skip results | Captured positions in #5061–#5064 | Captured in $AA_MW[axis] (work) / $AA_MM[axis] (machine) — readable only in Siemens mode. No CRC allowed in a G31 block |
| Block skip levels | / and /1 are the same switch | / and /1 are separate skip levels activated independently; levels /1–/9 available; skip sign works mid-block |
| M99 in a main program | Loops to program start | Same — but program runtime is not reset and the workpiece counter does not increment |
| Interrupts (M96/M97) | Enabled by parameter, UINT signal | Only work if MD10808 $MN_EXTERN_INTERRUPT_BITS_M96 bit 0 = 1; otherwise M96/M97 are treated as ordinary M-functions. Routed through cover cycle CYCLE396 by default |
| Comments | Parentheses | Parentheses work, and ; also starts a comment. Nested ( inside a comment keeps the comment open until every bracket is closed — can silently swallow the rest of the block |
| Optional codes | — | G51 scaling, G65/G66, G05.1, G07.1, G10, G68/G69, G72.1/G72.2 are flagged optional — presence depends on the machine builder |
Tapping note: whether F in G74/G84 is treated as feedrate (G94/G95 style) or as thread lead is a machine-data setting ($MC_EXTERN_FUNCTION_MASK bit 8) — verify before running a tapped hole from a Fanuc post.
Macro Support in ISO Mode (G65/G66 and the $C_ Variables)
G65 (non-modal) and G66 (modal, canceled by G67) call macros just like Fanuc — but the argument plumbing is entirely Siemens underneath. Every address programmed in the call block is stored in a system variable $C_A through $C_Z; I, J, K can be programmed up to 10 times per block and land in the arrays $C_I[0..9], $C_J[0..9], $C_K[0..9] (counts in $C_I_NUM etc.).
The critical restriction: transfer parameters can only be read in Siemens mode. If the macro’s first line is a PROC instruction, the control switches to Siemens mode automatically; without it, the macro body runs in ISO mode and must issue G290 itself before touching any $C_ variable. There is no Fanuc-style #1–#33 local-variable mapping and no ISO-mode IF/GOTO — conditional logic is written in Siemens syntax.
; Main program (ISO mode)
N30 G65 P10 F55 X150 Y100 S2000 ; call 0010.spf with arguments
; Macro 0010.spf written in Siemens mode
PROC 0010 ; auto-switch to Siemens mode
N10 DEF REAL X_AXIS, Y_AXIS, S_SPEED, FEED
N15 X_AXIS = $C_X Y_AXIS = $C_Y S_SPEED = $C_S FEED = $C_F
N20 G01 F=FEED G95 S=S_SPEED
N80 M17Two replacement mechanisms let ISO programs trigger custom routines the way Fanuc parameter 6050/6080 tables do: up to 50 G-numbers can call macros via MD10816/10817 $MN_EXTERN_G_NO_MAC_CYCLE(_NAME), and up to 10 M-numbers via MD10814/10815 (commonly used to hang a tool-change macro on M6). Only one replacement call per block; conflicts raise alarm 12722. The helper variables $C_TYP_PROG / $C_<addr>_PROG tell the macro whether each argument was programmed as integer or real — needed because of the decimal-point conversion factors above.
Run It in ISO Mode, or Translate?
If the program is straight posted CAM code — motion, canned cycles, cutter comp, work offsets, M98 subprograms — ISO mode will run it with minor cleanup (program-number file names, decimal-point machine data, cycle GUD settings). If the program leans on Fanuc Macro B — #-variables, IF/GOTO logic, probing math reading #5061 — there is no shortcut: that logic has to be rewritten in Siemens language anyway, so translate the whole program natively and skip the hybrid. Probing routines and tool-change macros are the usual tipping point.
References
- Siemens, ISO Milling Programming Manual, SINUMERIK 840D sl / 828D, 6FC5398-7BP40-3BA0, 02/2012.
Have a question or want to contribute?
Contact us with corrections, additions, or topics you'd like covered.
Get in Touch