DIN 66025 Subroutine Calls: Siemens vs Fanuc Reference

DIN 66025 Standard Scope and Subroutine Functions

DIN 66025 (the German Deutsche Industrie-Norm for numerically controlled machines) is the long-standing reference specification for the structure of NC programs, the format of preparatory functions (G-codes), miscellaneous functions (M-codes), axis addresses, and subroutine control. The standard is published in multiple parts:

• DIN 66025-1 – General structure of NC programs, word format, address characters, coordinate systems, and feed/spindle programming.
• DIN 66025-2 – Supplementary functions for machines with multiple slides, multiple spindles, and handling equipment (the so-called "class 6" functions that include M98 and M99).
• PAS 66025 / PAL – A pedagogical subset derived from DIN 66025, used in German vocational training programs (CNC milling/turning mechanic apprenticeships).

Bosch Rexroth documents its DIN 66025-compliant NC function set explicitly in the IndraMotion MTX programming manual, providing a working reference for class-6 functions and subroutine syntax. See the official Bosch Rexroth NC Functions per DIN 66025 manual (ID1866589).

Subroutine-Related M-Functions per DIN 66025-2

DIN 66025-2 defines miscellaneous (M) functions used for program-flow control on multi-slide, multi-spindle, and handling-equipped machines. The functions that govern subroutine calls and termination are listed below.

Siemens SINUMERIK Implementation

Siemens distinguishes explicitly between main programs (Hauptprogramme) and subprograms (Unterprogramme) at the file-system level. The naming convention is encoded into the program file extension and prefix.

Program Naming

Subroutine Call Syntax

; Modern SINUMERIK
L45 P03       ; Call subprogram SPF45 three times
; Older SINUMERIK
L56 P01       ; Call subprogram L56 once

; Modern SINUMERIK with program-name call
CALL "DRILL_45"   ; Symbolic call via NC program name

The P parameter specifies the repetition count. L45 P03 loads subprogram 45 and executes it three times before returning to the next block in the calling program.

Subroutine Termination

; Inside SPF45.SPF
...
M17            ; End of subprogram, return to caller (line after the L45 call)

; Or in main program
...
M30            ; End of main program, reset, rewind

Modal Subprogram Structure

SINUMERIK stores the calling block number and program pointer internally. M17 causes the controller to read these stored values and continue execution at the block immediately following the call. If the same SPF is called from multiple locations, the internal stack maintains up to 16 levels of nesting by default (parameter MD19250 / $MN_MM_MAX_SKB_DEPTH or similar, depending on SW version).

Fanuc Implementation

Fanuc does not distinguish between main programs and subprograms at the file-system level. All programs use the same prefix; the distinction is made by the M-function that terminates the program.

Program Naming

Fanuc uses the address O (the letter, not zero) for all program numbers, regardless of whether the program is a main program or a subroutine.

Subroutine Call Syntax

; Fanuc subprogram call
M98 P1234      ; Call subprogram O1234 once
M98 P1234 L5   ; Call subprogram O1234 five times (L = repeat count on Fanuc)

On Fanuc, the P word addresses the subprogram number; the optional L word specifies the repeat count. This is the inverse convention of Siemens, where L addresses the program number and P addresses the repeat count.

Subroutine Termination

; Inside O1234
...
M99            ; End of subprogram, return to block after the M98 P1234 call

; In main program O0001
...
M30            ; End of main program, reset, rewind

M99 has dual semantics on Fanuc: when used inside a subprogram it returns to the caller; when used at the end of a main program it acts as a loop-back, causing the controller to rewind to the beginning of the program and re-execute it. This dual role has no direct equivalent in Siemens syntax.

Syntax Comparison Table

Program Number Conventions and Address Conflicts

The address letters L and P have opposite meanings between Siemens and Fanuc. This is the single most common conversion error when porting NC code between controllers.

• Siemens: L = subprogram number, P = repeat count. Example: L45 P03 runs SPF45 three times.
• Fanuc: P = subprogram number, L = repeat count. Example: M98 P1234 L3 runs O1234 three times.

Program number ranges are also implementation-specific:

Reset Behavior and Modal State

The reset behavior at the end of a program, after an M30, or after a manual reset, is a critical difference between the two architectures.

PAL vs DIN 66025

PAL (Programmablauf or Programmier-Arbeits-Lehre, depending on the era) is a training-oriented subset of DIN 66025 used in German vocational curricula for CNC machining apprenticeships. The relationship between the two standards is summarized below.

The fact that the two are often cited together in classroom material leads to confusion when students encounter machines that implement only a subset of the standard. The class-6 functions (M98, M99) are explicitly not part of PAL and must be unblocked at the machine level before they can be programmed.

Bosch Rexroth MTX Implementation (DIN 66025-Strict)

The Bosch Rexroth IndraMotion MTX controller follows the Siemens convention but adds a clearly documented DIN 66025 mapping. Per the official programming manual, the following NC functions are exposed with DIN 66025 syntax.

The full function catalog is documented in the Bosch Rexroth NC Functions per DIN 66025 manual. When porting programs between Bosch Rexroth MTX and Siemens controllers, the syntax is generally interchangeable, but verify custom M-codes against the target machine's option list.

Verification Procedure

After converting or commissioning a DIN 66025 subroutine-based program, perform the following checks before running production parts.

1. Identify the controller platform. Read the HMI splash screen, the system-status page, or the machine-data screen to determine whether the control is Siemens (SINUMERIK 810/820/840C/840D sl/ONE), Fanuc (Series 0i/30i/31i/32i), Bosch Rexroth MTX, or Heidenhain. Do not assume compatibility based on the brand of the machine tool alone.
2. List the installed NC options. On Fanuc, press SYSTEM → PARAMETER → search for option-bit FSSB and macro-related parameters; confirm M98/M99 are enabled. On Siemens, check MD10715 / $MN_MM_LUD_VALUE_MEM and the option tree in the HMI for "subroutine expansion" or "class-6 M-functions."
3. Verify file-system naming. On Siemens, confirm the program file is stored as SPF<number>.SPF in the correct NC directory (typically /_N_CST_DIR/_N_SPF_DIR/ on HMI-Advanced, or under NC/Programs/Subprograms/ on SINUMERIK ONE). On Fanuc, verify the program is in the active program library under its O number.
4. Dry-run in single block. Set SINGLE BLOCK = ON (SBL on Fanuc, EINCBL on Siemens) and step through the program line-by-line, observing modal G-codes and modal M-codes in the status display.
5. Check call/return nesting. Set a higher single-block granularity (e.g., DEC1 on Siemens, SBK on Fanuc) and confirm that each M17 or M99 returns to the correct line in the calling program. Watch the block-counter and program-pointer displays.
6. Test reset behavior. While the subprogram is executing, press the Reset button and verify that the cursor returns to the expected position (main program on Siemens, last active program on Fanuc).
7. Repeat-count verification. Execute a call with a known repeat count (e.g., L10 P5) and verify that the subprogram runs exactly five times by counting a visible marker (e.g., a tool change or a probing event).
8. Production dry run. Run the program on a scrap part with DRY RUN (Siemens DRY, Fanuc parameter 1400 bit DRN) enabled at 50 % rapid feed to catch any modal-state issues.

Troubleshooting Matrix

Practical Field Notes

When retrofitting older machines or commissioning new installations, observe the following field-proven rules:

• Document the platform first. Place a header comment block in every program naming the controller type and software version. Siemens 840D sl behaves slightly differently across SW 4.x and 5.x regarding G-code reset values; Fanuc Series 0i-MF differs from 0i-TF in macro handling.
• Prefer M30 over M99 for main programs. M99-as-end-of-main is a common Fanuc pitfall; replacing it with M30 forces a clean rewind.
• Use absolute repeat counts. Avoid relying on modal repeat counts where the P/L argument is implied by a previous block. Always specify the count explicitly to make conversion easier.
• Keep nesting shallow. Restrict nesting to 3 levels or less to remain portable across controllers with hard limits.
• Test on the actual machine, not in the CAM simulator. CAM post-processors frequently emit "DIN 66025" syntax that is actually Siemens- or Fanuc-specific. The simulator may accept syntax the machine rejects (or vice versa).

FAQ