FANUC PS0206 Alarm: Cannot Change Plane During Rigid Tapping

FANUC PS0206 means that the program attempted to change the selected plane or drilling axis while rigid-tapping mode was active. On an applicable M-series control, this commonly occurs when G17, G18, or G19 changes the working plane before the rigid-tapping canned cycle has been canceled.

The official corrective direction is to modify the NC program. Keep one plane and one drilling axis throughout the active rigid-tapping cycle. If another plane is required, cancel the current cycle with the machine-approved canned-cycle cancellation command—normally G80—select the new plane, position the tool safely, and then establish a new rigid-tapping sequence with the required spindle speed and feedrate.

For the preceding signal alarm, see the FANUC PS0205 Rigid Mode DI Signal Off guide. For the broader list, see FANUC CNC Alarm Codes 0201–0400.

Safety Warning Before Retesting

Rigid tapping synchronizes spindle rotation with tapping-axis movement. Changing the plane changes how the CNC identifies the positioning axes and drilling axis. An incorrect plane, drilling direction, sign, depth, R point, S value, F value, or restart position can break the tap, damage the workpiece, or cause unexpected machine motion.

Record the original program, active modal state, alarm block, tool position, and machine setup before making changes. Verify the corrected sequence in the exact FANUC operator's manual and machine-builder programming manual. Test only under the machine builder's approved procedure and with qualified personnel present.

Do not restart directly from a G84 or G74 block after clearing PS0206. First restore the required plane, coordinate mode, feed mode, spindle selection, rigid-mode command, S value, F value, tool position, and other machine-specific modal conditions.

What Does FANUC PS0206 Mean?

FANUC alarm documentation describes PS0206 as plane changeover instructed in rigid mode. The program must be corrected so that the selected plane is not changed during the active rigid-tapping sequence.

The 0i-D machining-center user's manual expresses the same restriction in terms of the drilling axis: before the drilling axis can be changed, the canned cycle must be canceled. If the drilling axis is changed in rigid mode, PS0206 is issued.

These descriptions refer to the same programming relationship. In a standard M-series canned cycle, the selected plane determines the two positioning axes, while the remaining basic axis becomes the drilling or tapping axis. Changing from G17 to G18 or G19 can therefore change not only a geometric plane but also the axis along which the tapping cycle operates.

PS0206 is a program-state alarm. It does not mean that the CNC is unable to use G17, G18, or G19 under normal conditions. Those commands remain valid when they are used at an allowed point in the program. The prohibited action is changing the plane or drilling axis while the rigid-tapping cycle or rigid mode is active.

How G17, G18, and G19 Affect the Tapping Axis

For standard M-series canned-cycle programming, FANUC documents the following relationship:

The table uses the standard basic-axis relationship. A machine may also use axes parallel to X, Y, or Z, and multi-axis machines can have builder-specific restrictions. Confirm the exact drilling-axis selection rules for the installed CNC options and machine kinematics.

For a normal vertical machining-center tapping operation along Z, G17 is commonly selected before positioning and before the rigid-tapping request. If the program changes to G18 or G19 while the cycle remains active, the CNC sees a change in the positioning plane and drilling-axis relationship and can issue PS0206.

Do not confuse this rule with cutter-compensation plane alarms or an illegal circular-interpolation plane. PS0206 is specifically associated with a plane or drilling-axis change during rigid tapping.

1. Record the Active Plane and Alarm Sequence

Before editing the program, record several blocks before and after the alarm and identify:

• The complete FANUC CNC series, model, and software series

• Whether the control is configured as an M series or T series

• The active plane before the rigid-tapping command

• Every G17, G18, or G19 command around the tapping operation

• The rigid-mode M code used by the machine, commonly M29

• The active tapping cycle, such as G84 or G74 on an applicable M series

• The block that cancels the canned cycle

• The active feed mode, S value, F value, tapping depth, and R point

• Any macro, subprogram, CAM post processor, tilted working plane, indexing routine, or optional block involved

• Whether the alarm began after a program edit, post-processor update, parameter restore, CNC replacement, or machine modification

Check the modal display as well as the program text. G17, G18, and G19 are modal commands, so a plane selected earlier remains active until another plane is selected. The alarm block may be a G18 or G19 line, while the original G17 selection is located much earlier in the main program or a setup subprogram.

2. Select the Required Plane Before Entering Rigid Mode

For a Z-axis rigid-tapping operation on a standard M-series machine, select G17 before the rigid-mode command and keep it active through the cycle.

Example:

G17
G00 X50.0 Y30.0 Z5.0
M29 S500
G84 Z-20.0 R2.0 F1.25
X80.0 Y30.0
G80

The numerical values are examples only. The applicable feedrate depends on the feed mode and thread lead. Use the program format, spindle speed, feedrate, depth, clearance, and tool data approved for the actual machine.

The important structure is that G17 is established before M29 and remains unchanged until the tapping cycle is canceled. Repeated hole-position blocks can then use the same active plane and drilling axis.

3. Remove Plane Changes From the Active Tapping Cycle

An incorrect sequence may look like this:

G17
M29 S500
G84 Z-20.0 R2.0 F1.25
G18

The program attempts to select a different plane while the rigid-tapping cycle remains active. Move the plane change to a point after the cycle is canceled:

G17
M29 S500
G84 Z-20.0 R2.0 F1.25
G80
G18

This correction only establishes a legal point for the new plane selection. It does not by itself create a complete or safe side-tapping program. Before another rigid-tapping operation, reposition the tool and reissue the complete machine-approved rigid-mode, spindle-speed, feedrate, depth, and clearance sequence for the newly selected drilling axis.

Do not simply delete G18 or G19 if the next operation genuinely requires a different plane. First determine where the preceding canned cycle ends and reorganize the program so that the new operation begins from a fully canceled and verified state.

4. Cancel the Canned Cycle Before Changing the Drilling Axis

The 0i-D user's manual states that the canned cycle must be canceled before the drilling axis is changed. For the standard drilling-cycle G-code system, G80 is the normal cancellation command.

A safe program boundary is conceptually:

(First tapping operation on the current plane)
M29 S500
G84 ...
G80

(Select and prepare the next operation)
G18
G00 ...
M29 S___
G84 ...
G80

The second G84 block is schematic because the required axes and format depend on the control, machine, selected plane, options, and tool orientation. Do not copy it directly into a machine program.

On the 0i-D controls covered by FANUC B-64304EN-2/01, canceling the rigid-tapping canned cycle also clears the S value used for rigid tapping to S0. Therefore, do not assume that the previous rigid-tapping speed remains available after G80. Re-establish the required S value and rigid-mode sequence before the next tapping cycle.

The exact relationship between G80, the rigid-mode signal, and machine-builder PMC handling can vary by system. Use the verified cancellation procedure for the exact machine rather than using reset, emergency stop, or a forced PMC signal as a substitute for correct program structure.

5. Check Whether the Plane Actually Changes

FANUC's core wording refers to plane changeover or a change of drilling axis. A command that reselects the plane already active may not change the drilling-axis relationship on every control. However, software generation, machine options, or series-specific interpretation can make redundant plane commands difficult to diagnose.

When PS0206 occurs, inspect every G17/G18/G19 block inside the rigid-tapping section and compare each one with the active plane shown on the CNC. If a plane-selection command is redundant, remove it from the active cycle and place all required modal setup before the rigid-mode command. This produces a clearer program without claiming that every repeated same-plane command must trigger PS0206 on every FANUC control.

Do not change plane-initialization parameters merely to avoid a redundant command. The initial plane after power-up or reset can depend on CNC parameters and machine-builder configuration, but PS0206 is normally corrected by making the program's modal sequence explicit and legal.

6. Inspect Macros, Subprograms, and CAM Output

The visible main program may not contain an obvious plane change. Check the full execution path for:

• A tapping macro that includes G17, G18, or G19 as a setup line

• A subprogram shared by drilling, milling, and tapping operations

• A CAM post processor that repeats a safety line before every hole or toolpath

• A side-working or angle-head routine that selects a different plane

• Optional block delete that skips the intended G80 line

• A conditional macro branch that changes the plane only for certain holes

• Program restart that begins after the original plane selection or cycle cancellation

• A local subprogram that returns while the canned cycle remains modal

• A custom G code that expands into a plane-selection or drilling-axis command

A common post-processing problem is a generic safety block such as G17 G40 G80 being inserted at an unsuitable location. G80 may correctly cancel a canned cycle, but a G17/G18/G19 change placed before cancellation can still produce PS0206. Review the exact block order executed by the CNC rather than judging commands individually.

Compare the affected output with a known-good rigid-tapping program from the same machine. If the alarm began after a post-processor change, compare the generated code around every plane-selection, M29, G84/G74, and G80 block.

7. Account for M-Series and T-Series Scope

Classic FANUC Series 16i/18i/21i alarm tables and applicable spindle documentation label PS0206 as an M-series alarm. This matches the common machining-center use of G17, G18, and G19 to determine the positioning plane and tapping axis.

However, some later T-series operator manuals also state that the canned cycle must be canceled before the drilling axis is changed and that PS0206 can occur if the drilling axis is changed in rigid mode. T-series tapping cycles, plane conventions, rotary-tool functions, and G-code meanings can differ from M-series programming.

Therefore:

• Do not copy an M-series G17/G18/G19 example directly into a lathe program.

• Do not assume that every T-series control is exempt from PS0206.

• Confirm whether the machine uses G84/G74, G84/G88, a Series 10/11 format, a rotary-tool rigid-tapping option, or a builder-specific cycle.

• Use the exact operator's manual and machine-builder documentation for the CNC series, software, G-code system, and machine configuration.

This series limitation is also why two FANUC machines can react differently to programs that appear similar.

8. Do Not Start With Hardware, PMC, or Parameter Changes

FANUC's PS0206 corrective action is to modify the program. The alarm definition does not instruct the technician to replace the spindle amplifier, servo amplifier, motor, encoder, position coder, CNC main board, or feedback cable.

PS0206 also does not normally require changes to rigid-tapping gain, acceleration, backlash, maximum-speed, position-coder, spindle-selection, or plane-initialization parameters. A parameter or PMC review is appropriate only when the machine's documented cycle behavior, G-code system, drilling-axis configuration, or mode-cancellation sequence is genuinely uncertain—particularly after a CNC replacement, parameter restoration, retrofit, or ladder modification.

Do not force a rigid-mode signal OFF, bypass an interlock, or use reset as the normal way to move from one tapping plane to another. Correct the program boundary and verify that the cycle is canceled under the approved procedure.

Difference Between PS0204, PS0205, PS0206, and PS0207

For PS0206, begin with the NC program and modal state. Do not investigate the RGTAP DI signal merely because PS0205 is adjacent in the alarm list, and do not adjust distance-related data intended for PS0207.

FANUC PS0206 Diagnostic Table

Recommended Troubleshooting Order

1. Confirm PS0206 / CAN NOT CHANGE PLANE (RIGID TAP) and record the full alarm screen.

2. Identify the exact FANUC CNC series, software, M/T system, G-code system, machine model, and active path.

3. Record the active plane and drilling axis shown by the CNC.

4. Review the executed program from the plane-selection block through M29, G84/G74, repeated holes, and G80.

5. Locate every G17, G18, and G19 command in the main program, macros, subprograms, and post-processed output.

6. Keep the required plane selection before the rigid-mode command and do not change it during the active tapping cycle.

7. If another plane or drilling axis is required, cancel the current canned cycle before making the change.

8. After cancellation, reposition safely and reissue the required S value, F value, rigid-mode command, and tapping-cycle data.

9. Check optional block delete, conditional macros, custom G codes, and program restart for a skipped cancellation or hidden plane change.

10. Compare the program with a verified rigid-tapping program from the same machine.

11. Do not change parameters, force PMC signals, or replace spindle hardware without separate evidence.

12. Verify the corrected modal sequence in the exact FANUC and machine-builder manuals, then perform a controlled test.

Technical References

• FANUC Series 0i-MODEL D / 0i Mate-MODEL D User's Manual (Machining Center System), B-64304EN-2/01, rigid-tapping limitations, plane/drilling-axis relationship, G80 cancellation, and PS0206

• FANUC Series 0i-MODEL D / 0i Mate-MODEL D Connection Manual (Function), B-64303EN-1/01, rigid-tapping alarm list and CNC/PMC interface

• FANUC Series 16i/18i/21i Model B Operation and Maintenance Handbook, B-63527EN/01, PS0206 M-series alarm definition

• FANUC Series 0i-MODEL F Operator's Manual, B-64604EN-1/01, rigid-tapping axis-switching limitation for applicable M- and T-series functions

• FANUC Series 500i-A Maintenance Manual, B-64805EN/03, PS0206 alarm definition

• FANUC AC Spindle Motor and Servo Amplifier Maintenance/Parameter documentation, B-65280 series, PS0206 plane-change condition and M-series scope

• Beijing FANUC technical guidance for PS0206: cannot change plane during rigid tapping

Always use the manual edition that applies to the exact CNC, software, M/T system, G-code system, machine kinematics, tapping option, PMC, and machine-builder specification.

Need Help With FANUC PS0206 Alarm?

REACO CNC provides independent FANUC technical support, program review, drive testing, repair, and parts compatibility checking. Send us the PS0206 alarm screen, complete CNC and machine models, the program blocks from plane selection through G80, the active plane and drilling axis, and details of any recent program, post-processor, parameter, CNC, or machine changes.

Visit the FANUC Technical Support Center for more FANUC alarm guides, or contact REACO CNC for assistance.

Reference Source: Beijing FANUC. This article is based on FANUC technical documentation. The correct plane, drilling axis, tapping-cycle format, rigid-mode sequence, and cancellation procedure depend on the exact CNC, software, M/T system, machine, options, and machine-builder specification.