Siemens 840D Tool Compensation: Configuring OFFN, TOFFL, and L_39

Siemens 840D Tool Compensation: Configuring OFFN, TOFFL, and the L_39 Manufacturer Cycle

This technical reference consolidates field-proven practices for runtime tool compensation on Siemens 840D / 840D sl controllers, with emphasis on the DIN/ISO programming environment used on Deckel Maho DMC machining centers. It covers the OFFN, TOFFL, and TOFFR system variables introduced in SW 7.x, the manufacturer-specific L_39 subprogram, the PROG_EVENT.SPF reset hook, and the additive DL correction mechanism.

1. Compensation Strategies Overview

Tool compensation on a Siemens 840D can be performed at three distinct layers, and selecting the correct layer is the most common source of programming and operational issues:

For any correction that must be reversible on RESET or program interruption, system variables or additive DL corrections are strongly preferred. Direct writes to $TC_DP12 / $TC_DP15 persist in non-volatile tool memory and will survive power-cycle — a frequent cause of part scrap after weekend shutdown.

2. OFFN — Normal Offset (Contour Offset)

OFFN shifts the programmed contour normal to the path. It is active only while G41 or G42 cutter-radius compensation (CRC) is selected, and it works in the active machining plane.

Typical use cases:

• Radial stock allowance for finish-pass machining.
• Groove wall correction with TRACYL (where it differs from TOFFR).
• Compensating measured dimensional drift without touching tool wear.

Programmatic behavior:

; Apply 0.03 mm radial allowance
G0 X0 Y0 Z50
G41 G1 X10 Y0 F500 OFFN=0.03
; ... machining ...
OFFN=0            ; MUST be reset at end of operation
G40 X0 Y0         ; deselect CRC

OFFN is modal and additive to the active CRC. Forgetting OFFN=0 at program end is a documented cause of incorrect contour on the next workpiece, especially in mixed roughing/finishing programs.

3. TOFFL and TOFFR — Programmed Tool Offsets (SW 7.x)

TOFFL applies an additional length offset in the tool axis; TOFFR applies an additional radius offset. Both are write-only from the part program and are reset to zero on RESET / M30 / M6 by default. They were introduced with SW 7.0 and represent the recommended replacement for direct manipulation of $TC_DP12 / $TC_DP15.

3.1 Syntax Variants

Behavior comparison:

• Under normal conditions, TOFFR and OFFN produce identical results in the machining plane.
• For groove wall correction with TRACYL, TOFFR and OFFN diverge — use OFFN for cylinder-related groove compensation.
• All three (OFFN, TOFFL, TOFFR) are independent of tool-list wear data.

3.2 Ball-End Mill Reference Example

When a ball-end mill is automatically measured at the tip, but the CAM post-processor assumes the radius center, an axial offset equal to the negative radius is required:

; Ball mill D6, measured at tip, CAM assumes radius center
TOFFL = -3.0      ; D=6 → radius=3, so offset = -3 mm
; ... machining ...
TOFFL = 0          ; reset before tool change

4. The L_39 Manufacturer Cycle (Deckel Maho)

L_39 is a manufacturer cycle supplied by Deckel Maho (DMG MORI) on selected DMC machining centers. Its semantics mirror the Heidenhain DL/DR function:

L_39(REAL D_L, REAL D_R)

Where D_L is the length correction and D_R is the radius correction. Both may be positive or negative. The values are written into the wear fields of the active tool — not into a separate runtime variable. Calling L_39(0,0) zeroes both wear values for the active cutting edge.

4.1 Availability Matrix

4.2 Worked Program Excerpt

N18  MSG("SPHERE MILLING CUTTER D3")
N19  M6
N20  L_FREE
N21  G0 SUPA Z-1 D0
N22  G0 SUPA Y-1
N23  D1
N24  L_39(0.2,0)     ; OFFSET: L=0.2, R=0
N25  M0              ; operator confirms offset applied
...
N6750 D1
N6751 CYCLE800
N6752 L_39(0,0)      ; clear offsets before tool change
N6753 ;M91
N6756 M17

5. L_39 Source with Save/Restore Logic

The most robust pattern combines L_39 with GUD/U-GUD persistence and a PROG_EVENT.SPF hook. The example below reads the active tool's wear before the write and stores the deltas in user globals so the original wear can be reconstructed after a RESET.

5.1 GUD Definitions (UGUD.DEF or similar)

DEF CHAN INT  L_39_AKTIV      ; flag: correction active
DEF CHAN REAL KORR_D_L        ; original wear length at save time
DEF CHAN REAL KORR_D_R        ; original wear radius at save time

5.2 Modified L_39 Cycle

PROC L_39(REAL D_L, REAL D_R) SAVE DISPLOF
; VERSION: 1.0.0  Aug 28 2008
; Function: Fine adjustments to tool wear
; L_39(Length, Radius)
; L_39(0,0) restores the previously saved wear values

DEF REAL _DD

STOPRE
IF ($TC_MPP6[9998,1]==0) OR ($P_TOOL==0)
   ;msg("No tool or inactive tool in spindle")
ELSE
   IF L_39_AKTIV == 0
      ; first call: snapshot current wear
      KORR_D_L = $TC_DP12[$P_TOOLNO,$P_TOOL]
      KORR_D_R = $TC_DP15[$P_TOOLNO,$P_TOOL]
      _DD       = $P_TOOL
      L_39_AKTIV = 1
   ELSE
      ; second call with (0,0): restore
      D_L = KORR_D_L
      D_R = KORR_D_R
      L_39_AKTIV = 0
   ENDIF

   $TC_DP12[$P_TOOLNO,_DD] = D_L
   $TC_DP15[$P_TOOLNO,_DD] = D_R
   D = _DD
   STOPRE
ENDIF
M17

This pattern guarantees that wear is preserved even when the operator hits RESET mid-program. Three pre-allocated R-parameters can substitute for the GUD variables if GUD definitions are not permitted.

6. PROG_EVENT.SPF Reset Hook

The SINUMERIK program-event file PROG_EVENT.SPF (or the older CYCPE_MA.SPF) is invoked automatically by the NCK on specific lifecycle events. Two event codes are most relevant for tool compensation cleanup:

Minimum reset block:

IF (($P_PROG_EVENT==2) OR ($P_PROG_EVENT==3)) ; end or RESET
   ; delete fine corrections on active tool
   IF L_39_AKTIV == 1
      L_39(0,0)
   ENDIF
   TOFFL = 0
   TOFFR = 0
   OFFN  = 0
ENDIF

7. Alternative Correction Paths Without L_39

On Siemens controllers without L_39, three alternatives are field-standard:

7.1 OFFN for Radial Allowance

R99 = 0.03                     ; radial allowance
G41 G1 X10 Y0 F500 OFFN=R99
; ...
OFFN = 0
G40

7.2 $P_TOOLR for Single-Position Radial Approach

$P_TOOLR returns the active tool radius. For a single axis approach with compensation:

R99 = 0.03
G1 X=(10 - $P_TOOLR - R99) F500

7.3 TRANS Z= for Axial Offset

TRANS Z=0.05                  ; +0.05 mm in Z
; ...
TRANS                          ; clear all frames

TRANS is cleared by any subsequently programmed frame function, which is the main reason it is preferred only for short, isolated offset operations.

8. Additive Corrections (DL)

Additive corrections are tool-edge-specific offsets that are separate from the standard wear data. They are the cleanest method for in-process corrections because they are addressable by DL number and can be activated / deactivated without modifying the geometric tool data.

Typical flow:

D1 DL=1             ; activate D1 with additive correction 1
; ...
DL=0                ; deactivate additive offset

Additive DL data is entered through the HMI; the NC program only references the DL number. This separation makes DL corrections auditable and recoverable.

9. Recommended Pattern Selection

10. Troubleshooting Matrix

11. Field-Commissioning Checklist

1. Confirm NCK software version: >SWE> in the HMI — must be ≥ 7.x if TOFFL/TOFFR will be used.
2. Verify L_39 exists: open the cycles directory and search for L_39.SPF. If absent, fall back to OFFN/TOFFL.
3. Confirm PROG_EVENT.SPF is active: simulate RESET and observe whether the file is called ($P_PROG_EVENT reports 3).
4. Snapshot baseline wear for the test tool before the first L_39 run.
5. Run a single-part dry cycle; verify wear returns to baseline after M30.
6. Force a RESET mid-cycle; verify that all OFFN, TOFFL, TOFFR are zero and that wear is either restored or explicitly zeroed.
7. Document the chosen pattern in the cell setup sheet (operator-facing).

12. Related Siemens Documentation

• SINUMERIK 840D sl Programming and Operating Documentation — official Siemens Industry Online Support portal
• Programming Manual, Work Planning — section 9.2 "Additive Corrections" (referenced in field material; verify against the current manual revision)
• For a CNC-operator-level primer on cutter compensation concepts that underly these NCK mechanisms, see Autodesk Fusion 360: Cutter Compensation for Beginners.