FANUC PS0201 Alarm: Feedrate Not Found in Rigid Tap and Troubleshooting

FANUC PS0201 means that the CNC does not have a usable cutting feedrate for the rigid-tapping operation. The basic FANUC alarm description is that the required F command was not input. Depending on the CNC series and software, PS0201 can also be generated when the active F value is zero, is extremely small relative to the S command, or exceeds the permitted cutting-feed range.

The first correction is therefore to inspect the tapping program—not the spindle amplifier. Confirm that a valid F value is active and that it matches the selected G94 feed-per-minute or G95 feed-per-revolution mode, spindle speed, thread lead, input unit, and machine specification.

For the previous rigid-tapping alarm, see the FANUC PS0200 Illegal S Code Command guide. For the surrounding CNC alarms, see the FANUC CNC Alarm Codes 0201–0400.

Safety Warning Before Testing Rigid Tapping

Rigid tapping synchronizes spindle rotation with movement of the tapping axis. An incorrect feed mode or F value can produce the wrong thread lead, damage the tap or workpiece, or cause unexpected axis and spindle motion.

Do not test a modified tapping program directly in a production hole. Verify the CNC series, machine-builder programming method, tool data, spindle speed, thread lead, and units first. Use a controlled test condition approved by the machine builder and have the program checked by qualified personnel.

What Does FANUC PS0201 Mean?

FANUC spindle documentation for Series 16i and Series 30i lists alarm 201 or PS0201 as “F command is not inputted.” This is the clearest starting point: rigid tapping was requested, but the CNC did not receive a usable cutting-feed command for the synchronized tapping axis.

Later FANUC alarm documentation gives more detail. The Series 500i-A maintenance manual states that PS0201 is generated when the cutting feedrate commanded by F is zero. It can also be generated when F is extremely small compared with S, because the resulting programmed lead cannot be machined.

Some series use PS0201 for an additional range condition. For example, the cited 0i-F lathe manual states that an F value above the cutting-feed upper limit can cause PS0201. By comparison, the cited 0i-D machining-center manual assigns an excessive rigid-tapping F value to PS0011. Always use the alarm and programming manuals for the exact CNC series rather than assuming every FANUC control applies the same trigger conditions.

PS0201 is primarily a program or modal-state alarm. By itself, it does not indicate a failed spindle motor, encoder, feedback cable, spindle amplifier, or tapping-axis servo.

1. Record the Alarm Block and Machine Configuration

Before editing the program, record the block at which PS0201 appears and identify:

• The complete FANUC CNC series and model

• Whether the control is an M series or T series

• The active G-code system when applicable

• The rigid-tapping command, such as G84 or G74

• The machine-specific rigid-mode command, commonly M29 where required

• The active S and F values

• The active feed mode: G94/G95 or the equivalent for that control

• Whether G20 or G21 units are active

• The tap pitch, number of starts, and required thread lead

• Whether the values come directly from the program, a macro, or a subprogram

The machine builder can change the rigid-mode M code and program sequence. Do not assume that every FANUC-controlled machine uses exactly the same M29 format.

2. Confirm That a Valid F Command Is Active

Inspect the rigid-tapping block and the preceding modal program state. On the cited 0i-D machining-center system, the G84 format includes F as the cutting feedrate:

G84 X_ Y_ Z_ R_ P_ F_ K_ ;

Confirm that:

• An F value has been specified for the tapping cycle.

• The active F value is not zero.

• A macro variable used for F contains valid numeric data.

• The post processor did not omit F from the first tapping cycle.

• A subprogram or optional block did not replace F with zero or an unintended value.

• The decimal point and input units are correct for the control.

Canned-cycle data can be modal on applicable FANUC controls. A previous F value may therefore remain active during a sequence of holes, but relying on an old value makes troubleshooting and program review difficult. At the start of a new rigid-tapping operation, explicitly commanding the approved feed mode and correct F value makes the intended thread lead clear.

If no usable F command is active, correct the program. Changing spindle parameters or replacing hardware is not the official remedy for a missing feedrate command.

3. Confirm the G94 or G95 Feed Mode

For the 0i-D M-series programming convention cited here:

This distinction is essential. The same numeric F value has a completely different meaning in G94 and G95.

For example, a tap with a 1.5 mm lead at 500 min⁻¹ requires:

• In G94: F = 500 × 1.5 = 750 mm/min

• In G95: F = 1.5 mm/rev

If the program was calculated for G95 but G94 is active, or vice versa, the commanded lead can be wrong even though an F word is visible in the program.

Check the modal G-code screen as well as the program text. G94 or G95 may have been set in an earlier main-program block, subprogram, macro, or restart sequence.

Do Not Confuse M-Series G98/G99 With Feed Mode

On the M-series canned-cycle convention used in the cited 0i-D machining-center manual, G98 and G99 select the return level:

• G98: return to the initial level

• G99: return to the R-point level

They do not replace G94/G95 in that programming system.

On certain FANUC T-series G-code systems, however, G98/G99 can represent feed per minute/feed per revolution, while G94/G95 may be used in other G-code systems. This is why a tapping program copied between a lathe, machining center, or different G-code system must not be used without verification.

4. Calculate the Correct Rigid-Tapping Feedrate

Rigid tapping must maintain the programmed thread lead between spindle rotation and tapping-axis movement.

For feed per minute:

G94 F = spindle speed S × thread lead

For feed per revolution:

G95 F = thread lead

Use thread lead, not automatically the catalog pitch. For a single-start thread, lead equals pitch. For a multi-start thread:

Lead = pitch × number of starts

The inch example uses a lead of 1 ÷ 20 = 0.05 inch/rev. Confirm G20/G21, decimal-point behavior, and the permissible command resolution before entering the value.

The 0i-D manual provides the same relationship in its official example: at 1000 min⁻¹ with a 1.0 mm lead, G94 uses F1000, while G95 uses F1.0.

5. Check for F0, Empty Macro Data, or an Extremely Small Feed

If F is present but PS0201 remains, check how its value is produced. Common program-level findings include:

• F0 is commanded directly.

• A macro expression evaluates to zero.

• A variable has not been initialized before the tapping block.

• Unit conversion or rounding reduces the value to zero or below the usable command resolution.

• The program contains an F value that is extremely small relative to S.

• A post-processor setting outputs the wrong feed mode or insufficient decimal places.

The last condition has explicit support in the newer Series 500i-A alarm list: PS0201 can be generated when F is so small for the S command that the tool cannot cut at the programmed lead.

Do not simply enter an arbitrary larger F value. Recalculate the feed from the required thread lead and confirm that the result is permitted by the CNC and machine.

6. Check the Applicable Cutting-Feed Limit

The alarm used for an excessive F value differs by FANUC series and function:

If the calculated F is valid for the thread but exceeds the machine's permitted cutting feed, reduce the spindle speed and recalculate F while preserving the same lead. Do not change the thread lead merely to fit a speed selection.

Also confirm the maximum allowable feedrate in the machine-builder manual. A command accepted by the CNC is not automatically safe for the tapping axis, tool, holder, or workpiece.

7. Review Modal State, Subprograms, and the Post Processor

When the visible G84 block appears correct, trace the actual program path:

• Check whether G94/G95 was changed before the tapping cycle.

• Check whether a subprogram or macro changes F, S, G20/G21, or the feed mode.

• Confirm that an optional block containing the required F command was not skipped.

• Review the CAM post-processor output for the correct FANUC series and machine.

• After a program restart or manual edit, restate the required modal codes and tapping data according to the approved machine sequence.

• For a new tapping operation, avoid relying on feed data left by an unrelated drilling cycle.

FANUC states that drilling-cycle data is retained until modified or canceled on the cited 0i-D system. This explains why one group of holes may run using a modal F value even if later coordinate blocks omit F. It does not remove the need to define all required data correctly at the beginning of the cycle.

8. Run a Controlled Verification Test

After correcting the program:

1. Confirm the active unit system and G94/G95 mode.

2. Verify S, F, and the calculated thread lead.

3. Confirm the correct tap, holder, hole size, depth, and clearance.

4. Check that the rigid-tapping sequence matches the machine-builder procedure.

5. Perform a controlled test using an approved safe condition.

6. Confirm that PS0201 no longer appears and that the thread lead is correct.

FANUC warns that dry run and machine lock have specific behavior during rigid tapping. Do not assume these modes always keep spindle and tapping-axis behavior unchanged; follow the manual for the exact machine.

Difference Between PS0200, PS0201, and PS0207

PS0201 should not be used as a general description for every tapping-feed problem. If a nonzero F value is active and the CNC displays PS0207, diagnose the programmed lead and the exact control limits for PS0207 instead.

Difference Between PS0201 and PS0011

Both alarms can involve an F command, but they are not interchangeable:

Read the complete message and confirm the CNC model. The same program condition may not map to the same alarm number on every FANUC generation.

FANUC PS0201 Diagnostic Table

Recommended Troubleshooting Order

1. Confirm PS0201 and record the exact program block.

2. Identify the FANUC series, M/T system, G-code system, and machine-builder rigid-tapping method.

3. Confirm the active G20/G21 input unit.

4. Check that a valid nonzero F command is active for G84 or G74.

5. Check macro variables, subprograms, optional blocks, and post-processor output.

6. Confirm whether G94 or G95 is active on the applicable M-series system.

7. Calculate F from spindle speed and thread lead.

8. Verify that the calculated feed is within CNC and machine limits.

9. On a T-series control, confirm whether its G-code system uses G98/G99 or G94/G95 for feed mode.

10. Correct the program without changing unrelated spindle or servo parameters.

11. Perform a controlled test and verify the actual thread lead.

Technical References

• FANUC AC Spindle Motor αi/βi Series Parameter Manual, B-65280EN/08, rigid-tapping program alarm list for Series 16i and Series 30i

• FANUC Series 0i-MODEL D / 0i Mate-MODEL D User's Manual (Machining Center System), B-64304EN-2/01, rigid tapping, G84/G74, F-command units, G94/G95 examples, and thread-lead relationship

• FANUC Series 0i-MODEL F Operator's Manual (Lathe System), B-64604EN-1/01, rigid-tapping F-command limit and T-series feed-mode codes

• FANUC Series 500i-A Maintenance Manual, B-64805EN/03, PS0201 alarm conditions for F0 and an extremely small F-to-S relationship

• Beijing FANUC technical guidance for PS0201: feedrate not commanded during rigid tapping

Always use the manual edition for the exact CNC series, machine type, G-code system, software, and machine-builder configuration. Alarm wording, feed-mode codes, valid command ranges, and rigid-tapping sequences can differ.

Need Help With FANUC PS0201 Alarm?

REACO CNC provides independent FANUC technical support, program review assistance, drive testing, repair, and parts compatibility checking. Send us the alarm screen, complete CNC model, tapping program around the alarm block, active modal G codes, S and F values, thread specification, and machine model.

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

Reference Source: Beijing FANUC. This article is based on FANUC technical documentation. The correct program and test procedure depend on the exact CNC, machine, G-code system, spindle configuration, and machine-builder specification.