G291 ISO Mode – Haas Program Compatibility on SINUMERIK ONE

G291 switches the SINUMERIK control into ISO dialect mode, allowing it to interpret programs written in Haas- or Fanuc-style G-code without converting them to native Siemens syntax

When active, ISO mode:

• Accepts only ISO dialect G/M codes; Siemens-specific G/M codes cannot be used.
• Retains the currently active tool, tool compensation, and work offsets when switching between G290 and G291.
• Prevents mixing Siemens and ISO commands in the same program block.
• May automatically switch to Siemens mode during certain calls (see Subprograms & Macros section).

For complete syntax rules, function limits, and safety guidance, consult the manuals listed in the References section before running in production.

To enter ISO dialect mode:

• G291 ; Enable ISO dialect NC programming language

To return to native Siemens mode:

• G290 ; Enable Siemens NC programming language

Rules:

• G290 and G291 must be the only command in their program block.
• Switching modes does not clear the active tool or offsets.
• Mode switching is per channel, one channel can run in ISO while another remains in Siemens mode.

In G291 ISO mode, the control accepts Haas-style tool commands, but you must specify both the tool (T) and the length/diameter offset (D) to have the correct values applied from the tool table.

ISO Mode Tool Change Syntax

T1 M6                ; Changes tool to Tool 1, no offset applied
T1 D1 M6              ; Changes tool to Tool 1 and applies Length/Radius Offset 1

Important:

• The T and D values must exist in the tool table for the offset to be applied.
• If only T is specified (e.g., `T1 M6`), the tool changes but no length/diameter offset is active.

Native Mode Tool Call (G290)

In G290 native Siemens mode, use `TOOLCALL`:

TOOLCALL 1 D1         ; Calls Tool 1, applies Length/Radius Offset 1

Notes:

• `TOOLCALL` cannot be used in ISO mode (G291). Attempting to do so will result in a syntax error.
• Tool changes in Siemens native mode apply offsets automatically if specified in the `TOOLCALL` line.
• Always confirm the correct offset is active in the tool table before machining.

Work coordinate offsets define the machine position of the workpiece zero. In ISO mode (G291), SINUMERIK interprets standard G54–G59 offsets the same way Haas or Fanuc-based controls do.

• G54 to G59 — Standard work offsets (same as Haas/Fanuc)
• G505 to G599 — Extended work offsets (if enabled by machine data)
• G500 — Resets all applied offsets (returns to machine coordinate system)

G291            ; Enter ISO Mode
G54             ; Use Work Offset 1
T1 D1 M6        ; Load tool and offset
G0 X0 Y0        ; Move to work zero

SUPA – Suppresses all offsets (tool, work, and measurement).

Not available in ISO mode — use G500 instead.

Note: `SUPA` is not supported in G291 ISO mode. Use `G500` to reset the work offset instead.

• Always define offsets in the Zero Offset table before use.
• ISO programs start with the active work offset from the previous program unless changed.
• Use G500 before setting a new G54–G59 if you require a clean state.

• Always include an explicit `G54` (or G55/G56...) call early in your ISO program, do not assume it's carried from the previous program.
• Avoid using `SUPA` in G291. Use `G500` to clear work offset and return to machine coordinates.
• When switching between Siemens native and ISO modes, reapply the appropriate offset (e.g., `G54` in ISO, or `G54` + `TOOLCALL` in native).

In G291 ISO mode, the control accepts standard Haas canned cycles (G81–G89, G73, etc.) directly and interprets them using ISO shell cycles. You do not need to rewrite them unless you are converting the program to run in native Siemens mode (G290).

When using G290, Haas cycles must be rewritten to the equivalent Siemens `CYCLE..` format. Siemens cycles are functionally similar but require parameters inside parentheses, separated by commas.

Example conversion to native Siemens:

Haas:    G83 Z-1.0 R0.1 Q0.2 F5.0
Siemens: CYCLE83(1.0, 0.1, 0.0, 0.2, 5.0)

Notes

• In G291, run Haas cycles as-is.
• In G290, rewrite to the `CYCLE..` format.
• For left-hand tapping in native mode, include `M4`.
• G73 has no direct Siemens cycle and must be emulated with a subprogram or PROC.

Haas uses custom macros to handle logic, loops, and variables. These typically rely on:

• `#` variables (e.g., `#101 = 5.0`)
• Macro calls using `G65`
• Conditional logic (e.g., `IF`, `GOTO`)
• Local/Global variable scopes

Example (Haas):

#101 = 5.0
G65 P9001 A#101
IF [#101 GT 10] GOTO 100

Siemens handles logic using structured programming with:

• `R` variables (e.g., `R1 = 5.0`)
• Subprogram calls using `LBL`, `CALL`, or `PROC`
• `IF`, `WHILE`, `GOTO`, `ENDWHILE` logic blocks
• Local vs Global variable declarations

Example (Siemens):

R1 = 5.0
CALL LBL1
IF (R1 > 10)
  GOTO LBL100
ENDIF

Note: Siemens macros do not work while `G291` ISO mode is active. `G291` is for standard G-code interpretation only. To use macro logic, you must switch back to native Siemens mode with `G290`.

• Avoid placing macro logic inside `G291` sections.
• Use `TOOLCALL`, `CYCLE`, and native Siemens logic outside `G291` for full compatibility.
• Rebuild Haas macros using Siemens `PROC` subprograms if needed.

Haas probing G-codes (WIPS) are thin wrappers around macros that drive a probe using skip motion (G31), then write results into work offsets. On SINUMERIK you can:

• Stay in G291 (ISO) and program raw probing with G31, then write offsets with G10.

• Switch to G290 (native) and call Siemens measurement cycles / MEAS instructions to do the same job with guided masks.

• G31 (skip) in ISO works the same conceptually: feed until probe triggers, stop at hit.

• In G291, write offsets programmatically (G10 write).

• In G290, use Siemens measurement cycles / MEAS / MEASA / MEAW; they handle trigger & offset writes.

Safe header for any raw probing block

G90           ; absolute
G94           ; feed per minute
G21 (or G20)  ; units match program
F500          ; safe probing feed (e.g., 500 mm/min or 20 ipm)

G94
F500
G31 X#<_target>    ; stop on hit, position latched
; compute offset, then:
G10 L2 P1 X#<_wcs_x> Y#<_wcs_y> Z#<_wcs_z>

(single X-face example)
G94 F500
G31 X[#<_approach>]    ; approach toward face
; math → X0 at hit ± stylus radius
G10 L2 P1 X#<_newX>    ; write G54 X

(two touches)
G94 F500
G31 X[#<_approachX>]
G31 Y[#<_approachY>]
; math → corner coords
G10 L2 P1 X#<_newX> Y#<_newY>

(4 touches @ 0/90/180/270)
G94 F500
G31 X+... ; +X touch
G31 X-... ; -X touch
G31 Y+... ; +Y touch
G31 Y-... ; -Y touch
; math → center & diameter
G10 L2 P1 X#<_cx> Y#<_cy>

(two parallel faces)
G94 F500
G31 X+...
G31 X-...
; math → width & midline
; optionally update offset:
G10 L2 P1 X#<_centerX>

(example: length touch)
G94 F200
G31 Z-...    ; descend to setter, stop on trigger
; compute/meas length → write to tool table

• Commissioning: G31 requires the probe’s skip input to be mapped in the PLC. If a G31 move never “hits,” that’s a wiring/commissioning issue.

• Units & feed mode: Force G94 for consistent F behavior (especially on lathes that often run G95).

• Offset writes in ISO: G10 write syntax follows the ISO dialect (e.g., `G10 L2 P<offset> X.. Y.. Z..` for G54..G59). Confirm dialect & axis sign per your setup.

• Mode swaps: If you switch to G290 to use Siemens cycles, keep G290 and G291 on their own lines. Re-assert any needed frames/offsets after swapping.

• Operator control: Using G1 for approach lets the operator scale speed with feed-override (useful on first-article runs).

• Safety: Start with generous clearance planes and conservative feeds; verify probe calibration before writing any WCS or tool data.

If your incoming Haas code uses G291 for half-rapid, replace it with a short, scoped feed block:

(HAAS G291 → Siemens-safe slow approach)
G94
F500
G1
; ... sensitive moves only ...
G0

YouTube: ISO compatibility mode with G291 in Turning

Mr. CNC covers running ISO-based G-code (RS-274) on SINUMERIK using G291 — including enabling/disabling ISO mode (G291/G290), tool call formats for lathes and mills, subprogram handling, mixing DIN/ShopTurn/ISO code, differences on 808D, and key limitations such as loss of certain Siemens functions.

SINUMERIK 840D sl / 828D / 802D sl – ISO Dialects, Function Manual

• Edition: 07/2022 Order No.: A5E52211448 B AA
• Covers: ISO G-code interpretation (e.g., G291/G290, G/M codes, cycles, tool offsets in ISO mode).

SINUMERIK ONE – NC Programming Manual

• Edition: 03/2025 Order No.: A5E48054250B AK
• Covers: Native SINUMERIK programming (e.g., TOOLCALL, work offsets G54–G599, G500, SUPA, cutter compensation, structured programming, PROC, G290).

SINUMERIK 840D sl / 840D / 840Di sl / 840Di / 810D – Cycles Programming Manual

• Edition: 04/2006, Order No. 6FC5398-3BP10-0BA0
• Covers: Full breakdown of CYCLE81 through CYCLE959, including syntax, parameters, and usage examples for drilling, milling, and turning.