Resolving SINUMERIK C-Axis Positioning Errors After Drilling

Resolving SINUMERIK C-Axis Positioning Errors After Drilling Cycles

Problem Overview

Operators running DMG MORI multi-axis turning-milling machines with Siemens SINUMERIK 840D sl controllers frequently encounter alarm conditions when attempting to position the C-axis immediately after a drilling cycle completes. The typical symptom is the NC refusing to index the spindle to a new angular position, returning an alarm that indicates no valid transformation or positioning block can be executed at this point in the program.

This is a documented behavior of the SINUMERIK kinematics model. Standard drilling cycles do not implicitly activate a frame or transformation, and they do not force a defined spindle position state at cycle exit. When the C-axis is commanded to rotate to a new angular coordinate while the controller still has a milling-mode transformation active (commonly TRANSMIT, TRACYL, or TRAORI), the NC raises an alarm because C-axis indexing requires a consistent kinematic state with the spindle in pure axis mode.

Root Cause: Transformation State Conflict

The SINUMERIK distinguishes between three operating modes for the main spindle on a turning-milling machine:

1. Spindle mode — rotational speed control, controlled through M3, M4, M5, and S.
2. Axis mode — DC-coupled, position-controlled, addressed through the C-axis name or through SPOS / M70.
3. Interpolated mode — combined with linear axes through an active transformation (TRANSMIT, TRACYL, TRAORI).

Standard drilling cycles (CYCLE81, CYCLE82, CYCLE83, CYCLE84, CYCLE85, CYCLE86, CYCLE87, CYCLE88, CYCLE89) operate inside the active coordinate system. If a TRANSMIT or TRAORI transformation is active at the time the cycle starts, the cycle executes inside that transformed space and the C-axis remains implicitly coupled. After the cycle ends the transformation is not automatically deactivated. A subsequent C-axis indexing command issued without first deactivating the transformation triggers alarm 14092 or 14093 depending on the installed firmware revision.

The header bar of the SINUMERIK HMI displays the currently active transformation, plane, and frames at all times. On DMG MORI machines running CELOS the same status information is available through the SINUMERIK diagnostics view inside the CELOS Documents pane. This is the first location to verify the kinematic state before issuing a positioning command.

Diagnostic Procedure

Follow this sequence to identify the active kinematic state before commissioning the C-axis move:

1. Switch the controller to JOG mode.
2. Press the HELP key on the HMI. The system lists every PDF manual installed on the controller.
3. Navigate to the active G-code program. The header line above the program window shows the active transformations, frames, and plane selection.
4. On DMG MORI machines with CELOS, open the Documents application. The Siemens programming and operating manuals for the installed SINUMERIK version are available there as PDFs.
5. Confirm whether TRANSMIT, TRACYL, or TRAORI appears as active.
6. If a transformation is active, note whether the current spindle position is being driven as a coupled C-axis or as a free spindle.

Solution: Deactivate the Transformation with TRAFOF

The standard remedy is to deactivate the active transformation explicitly using the TRAFOF command before issuing any C-axis positioning move that must take place in the machine coordinate system rather than the transformed system.

; --- Step 1: drilling cycle with active TRANSMIT ---
TRANSMIT
G0 X50 Z2
CYCLE83(50, 0, 2, -15, , 3, 0.5, 0, 0, 0, 90, 0)

; --- Step 2: explicitly deactivate the transformation ---
TRAFOF

; --- Step 3: index the C-axis in plain spindle mode ---
SPOS = 90

; --- Step 4: continue with subsequent operations ---
G0 X100

If the machining sequence contains a turning operation between the drilling cycle and the C-axis positioning move, the controller deactivates the milling-side transformation automatically because the active cutting mode switches from milling to turning. This is why an intermediate turning pass can serve as an implicit TRAFOF. The behaviour is real but fragile and depends on the cycle configuration. The explicit TRAFOF approach is preferred for production code.

C-Axis Operation Fundamentals

The C-axis on a turning-milling machine is implemented by closing the position loop on the spindle motor encoder. Two implementation variants exist, documented in the Siemens C-Axis Function Manual:

In both cases the spindle transitions between speed control and position control through the M70 command or the equivalent SPOS command with a target position. The functional difference matters for the achievable dynamics and for the firmware-level commissioning parameters, not for the G-code interface.

When the C-axis is positioned through SPOS the spindle comes to rest at the commanded angle. SPOSA performs the same function but defers the position stop to the next NC block boundary, which is the mechanism used for drilling on-the-fly with coordinated axis motion.

; Position C-axis to 90 degrees with explicit block transition
SPOS = 90

; Position C-axis with deferred stop (drill while moving)
SPOSA = 180

Drilling Cycles and Transformation Interaction

The SINUMERIK ShopMill and ShopTurn cycle masks expose the C-axis through the "Positioning" input field. Internally the cycle generates an SPOS block when needed. The cycle does not generate a TRAFOF or TRAORI command. The transformation must already be in the correct state when the cycle is called.

For cycles that require spindle positioning (CYCLE84, CYCLE85, CYCLE86) the operator must confirm that the spindle is in axis mode (M70 issued, or SPOS programmed at least once) before the cycle starts. The cycle mask exposes this through the "Spindle stop" toggle in the parameter screen.

Verification

After inserting the TRAFOF command, verify the fix through the following checks:

1. Run the modified program in Single Block (SBL) mode.
2. Confirm the G-code listing header shows no active transformation after the TRAFOF block executes.
3. The C-axis should move to the commanded angle without alarm and with the spindle in axis mode.
4. Check the active kinematic state through the Axis diagnostics screen on the HMI. The spindle section should show Axis mode active.
5. Run the program in AUTO mode with reduced rapid override (25%) before production release.

Accessing Siemens Documentation on the Machine

DMG MORI machines running SINUMERIK controllers provide the official Siemens documentation through two paths:

• HELP key in JOG mode: Press the HELP key while the controller is in JOG mode. The system displays the manuals installed on the controller. Search for the cycle name (e.g. "CYCLE83") or the function keyword (e.g. "TRANSMIT") to access the relevant programming manual section.
• CELOS Documents pane: On DMG MORI machines with the CELOS HMI, the Documents application contains the Siemens programming and operating manuals as PDFs, indexed by part number and software version.

External download is available from the Siemens Industry Online Support portal. Search for the controller part number (e.g. 6FC5370-AA00-0AA0 for SINUMERIK 840D sl) to locate the matching programming manual.

Common Pitfalls

• Implicit transformation in cycle call: Some ShopMill and ShopTurn cycles wrap the user code in a TRANSMIT block. Inserting TRAFOF inside the cycle call has no effect because the wrapper re-activates the transformation on cycle exit.
• Frame persistence: Active frames (ROT, AROT, TRANS, MIRROR, SCALE) survive TRAFOF. They must be cleared separately with ROT, AROT, or TRANS issued without parameters.
• Plane change: G17 / G18 / G19 affects the drilling cycle plane interpretation. It does not affect C-axis positioning but can cause intermittent alarms if the plane is inconsistent with the active transformation.
• Block search: Use SERUPRO mode for block search with transformation changes. A standard block search can leave the controller in an inconsistent kinematic state because the search skips over the TRAFOF block.
• Modal C-axis switch: Issuing SETMS(n) to switch the master spindle does not deactivate the active transformation. Verify the state after any spindle swap.

Production-Ready Programming Template

; ============================================
; Multi-axis drill-and-index sequence
; Tested on DMG MORI CTX beta 1250
;   with SINUMERIK 840D sl SW 4.7 SP3
; ============================================

G18 G54              ; Select turning plane, set work offset
TRANS Z2.5           ; Shift zero by Z2.5 mm

; --- Drill first hole at C=0 ---
TRANSMIT
G0 X50 Z2
CYCLE81(10, 0, 2, -8)

; --- Index to next angle ---
TRAFOF               ; Deactivate transformation
SPOS = 60            ; Rotate C-axis to 60 degrees
M70                  ; Ensure axis mode (redundant with SPOS)
TRAFOF               ; Idempotent safety call

; --- Drill at C=60 ---
TRANSMIT
G0 X50 Z2
CYCLE81(10, 0, 2, -8)

; --- Repeat pattern as needed ---
TRAFOF
SPOS = 120
TRAFOF

TRANSMIT
G0 X50 Z2
CYCLE81(10, 0, 2, -8)

; --- Final cleanup: deactivate, return to spindle mode ---
TRAFOF
SETMS(1)
M30

The second TRAFOF call after each SPOS is intentional. TRAFOF is idempotent and protects against a transformation being reactivated by a cycle mask configuration the operator has forgotten.

Related Siemens Commands Reference

Safety Notes

For drilling operations that combine C-axis rotation with linear interpolation (helical drilling, circle milling around a bore), keep the spindle in transformed mode and use SPOSA rather than SPOS to coordinate the position stop with the linear motion. Switching to plain spindle mode mid-helix will desynchronise the interpolator.

Troubleshooting Matrix