G04 Dwell Command Guide: Fanuc, Siemens, and Mitsubishi

Introduction

An unexpected tool drag across a semi-finished workpiece, a sudden spindle stall, or witness marks scarred into a critical sealing surface—each of these production-halting events points back to a failure in programming the G04 dwell command. While a dwell is designed to temporarily suspend axis motion, a simple parameter mismatch or an improperly configured unit of time can cause a CNC machine to resume interpolation prematurely. In high-precision turning and milling, understanding the exact mechanical consequences of G04 behavior is the difference between achieving a mirror-like finish and throwing the machine into an immediate emergency alarm state.

Technical Summary

Technical Specification	Value / Details
Command Code	G04 / G4
Modal Group	Group 00 (Non-modal)
Supported Brands	Fanuc, Siemens, Mitsubishi
Critical Parameters	Parameter 3405 DWL (Fanuc), MD20734 bit 2 (Siemens), Parameter #8130 (Mitsubishi)
Main Constraint	Interrupts continuous-path mode smoothing, must be programmed alone in a block on Siemens, can trigger alarm PS0041 on Fanuc when cutter compensation is active.

Quick Read

• Verify Feed Mode: Always check if feed per minute (G94) or feed per revolution (G95) is active, as brand parameters can dynamically switch the dwell unit from seconds to spindle revolutions.
• Avoid Deceleration Marks: Do not insert G04 during smooth surfacing passes (G64/G641 on Siemens) to prevent the tool from decelerating to a dead stop and leaving witness marks.
• Format Address Correctly: Use explicit decimal points for time-based addresses (like X or U) to bypass mathematical scaling or integer interpretation errors.
• Ensure Separate Block Execution: Write G04 alone in its own NC block on Siemens controls to avoid immediate G-code block errors (Alarm 12120).
• Cutter Compensation Limit: Never program consecutive non-movement blocks like G04 during active cutter radius compensation (G41/G42) to prevent path-blending failures (Alarm PS0041).
• Spindle State Check: Verify that the spindle is actively rotating before executing a revolution-based dwell under G95 mode to prevent an infinite program hang.

Basic Concepts

The primary practical programming effect of the G04 command is an intentional pause of all physical axis interpolation for a specified time or a calculated number of spindle rotations. CNC programmers use this temporary suspension of tool movement to clear chips, allow the spindle to reach its commanded velocity, or wait for external mechanical operations to complete. By forcing the tool axes to remain stationary while the spindle continues to spin, the command ensures that subsequent cuts begin from a steady, controlled state.

However, because G04 is a non-modal command belonging to Group 00, it is only active in the specific block where it is written. Once the dwell duration is satisfied, the controller immediately resumes normal axis interpolation in the subsequent blocks. The transition from stationary standby back to active feedrate requires careful synchronization, especially when machining critical features where even a fraction of a second of premature tool movement can lead to workpiece defects or severe tooling wear.

Command Structure

To execute a dwell command, the G04 code is followed by a specific address character that designates the duration or count of spindle revolutions. Programmers must select the correct address character—typically P, X, U, F, or S—depending on the active control system and the desired unit of measurement. The mathematical interpretation of these addresses is highly dependent on system-level parameter settings, which can scale integer inputs by several decimal places or dictate whether a decimal point is even accepted.

Furthermore, the G04 command behavior varies depending on whether it is programmed in a time-based mode or a spindle revolution-based mode. In time-based mode, the axes pause for a precise period of seconds or milliseconds, which is ideal for allowing hardware states to settle. In revolution-based mode, the axis pause is directly synchronized with the encoder of the spindle, meaning the dwell terminates only after the spindle has rotated a specified number of times, which is essential for uniform cutting and chip-breaking.

; Fanuc Syntax
G04 P_ ;
G04 X_ ;
G04 U_ ;
G04 X(U, P)_ Q_ ;
; Siemens Syntax
G4 F_ ;
G4 S_ ;
G4 S<n>=_ ;
G04 X_ ;
G04 P_ ;
; Mitsubishi Syntax
G94 G04 X_ ;
G94 G04 P_ ;
G94 G04 U_ ;
G95 G04 X_ D_ ;

Brand	Parameter	Functional Description	Valid Range / Bits
Fanuc	Parameter 3405 bit 1 (DWL)	Dictates dwell execution: 0 = always seconds; 1 = seconds in G94, spindle revolutions in G95.	0 or 1
Fanuc	Parameter 1020 bit 7 (DWT)	Determines P address increment system: 0 = active increment system (e.g., 1 ms for IS-B); 1 = locks unit to 1 millisecond.	0 or 1
Fanuc	Parameter 8002 bit 1 (DWE)	Specifies minimum dwell programmed time in PMC axis control under IS-C: 0 = 1 ms; 1 = 0.1 ms.	0 or 1
Siemens	MD20734 $MC_EXTERN_FUNCTION_MASK bit 2	In ISO Dialect mode: 0 = always seconds/milliseconds; 1 = seconds in G94/G98, spindle revolutions in G95/G99.	0 or 1
Siemens	MD11411 $MN_ENABLE_ALARM_MASK bit 7	Enables stop delay area warning Alarms 16954 and 16957.	0 or 1
Siemens	MD11550 $MN_STOP_MODE_MASK	Defines the system-level stop delay area boundaries.	System dependent
Mitsubishi	Parameter #8112 DECIMAL PNT-P	Determines if a decimal point is valid in the P address: 0 = ignore decimals; 1 = validate decimals.	0 or 1
Mitsubishi	Parameter #19014 G04 P factor	Scales the P address integer (without decimal) by a multiplier of 10<sup>n</sup>.	-3 to 3
Mitsubishi	Parameter #1173 dwlskp	Defines the PLC interface skip input signal combination (Skip 1 to Skip 3) to abort dwell.	0 to 7
Mitsubishi	Parameter #8130 Dwell in rev.	Determines dwell type in synchronous feed (G95) mode: 0 = time-based (seconds); 1 = spindle revolutions.	0 or 1

Brand Applications

Fanuc

In the Fanuc control ecosystem, G04 serves as a precise non-modal tool to suspend axis interpolation. Programmers must configure parameter 1020 bit 7 (DWT) and parameter 3405 bit 1 (DWL) to control whether the P address acts as a rigid millisecond value and whether G04 transitions to spindle revolutions in G95 mode.

Standard G-code syntax supports G04 P_, G04 X_, or lathe-specific G04 U_. When the multi-stage skip option is active, the syntax is expanded to G04 X_ Q_ or G04 P_ Q_, enabling external PLC signals to abort the dwell.

• Parameters: Parameter 1020 bit 7 locks P to 1 ms. Parameter 3405 bit 1 enables revolution-based dwell in G95 feed. Parameter 8002 bit 1 controls the minimum time increment under PMC axis control.
• Alarms: Alarm PS0041 triggers during cutter compensation (G41/G42) if multiple non-movement blocks occur. Alarm PS0370 triggers if the programmed Q address is outside the 1 to 4 (or 1 to 8) range. Alarm PS0373 triggers if duplicate high-speed skip signals are selected in multiple paths.
• Versions: Lathe (T-series) natively supports the incremental U address for dwell, whereas M-series controls primarily restrict dwell to X and P. High-speed continuous skip options extend the Q address range from Q1 to Q8, compared to the standard Q1 to Q4 limit.

Warning: Stringing together consecutive dwell blocks or auxiliary commands while cutter compensation is active can confuse the path look-ahead vector, leading to an immediate PS0041 tool interference alarm.

Siemens

Native Siemens controls implement the dwell command using G4 syntax, requiring the command to reside strictly in its own NC block. Programmers utilize machine data MD20734 bit 2 to determine if the G4 command dynamically switches from seconds to spindle revolutions based on active G94/G95 feed modes.

In native Sinumerik mode, G4 accepts G4 F_ for time in seconds and G4 S_ for revolutions. In addition, the unique G4 S<n>=_ syntax allows the dwell to synchronize specifically with secondary spindle revolutions, while G291 ISO Dialect mode converts the syntax to G04 X_ or G04 P_.

• Parameters: MD20734 bit 2 enables feedrate-dependent dwell units in ISO mode. MD11411 bit 7 switches on stop delay area warning alarms. MD11550 defines the physical stop delay area boundaries.
• Alarms: Alarm 12120 triggers if auxiliary M-codes or G-functions are programmed in the same block as G4. Alarm 16954 or 16957 is thrown if an operator attempts a programmed stop at 0 override inside a stop delay area. Mechanical status timeouts generate clamping Alarms 700011, 700013, or 700022.
• Versions: Switching between native Siemens mode (G290) and ISO Dialect mode (G291) alters G4 addresses from F/S to X/P. In native mode, specific spindle revolutions are designated inline, while ISO mode uses parameter-based feedrate tracking.

Warning: Never program coolant codes or auxiliary M-functions in the same block as a G4 dwell command, as the Sinumerik parser will instantly stop execution with a block syntax Alarm 12120.

Mitsubishi

Mitsubishi systems offer robust G04 standby logic that tightly integrates axis pauses with PLC hardware states. Programmers rely on parameter #8130 to dictate if the dwell adapts to spindle revolutions in G95, and configure parameter #8112 to validate decimal points.

Syntactically, Mitsubishi supports G04 X_, G04 P_, and lathe-specific G04 U_ formats. For revolution-based pauses, appending a D address like G04 X_ D_ links the dwell to a designated spindle encoder.

• Parameters: Parameter #8130 enables revolution-based dwelling in G95. Parameter #8112 validates decimal inputs in the P address. Parameter #19014 scales integer-only P values. Parameter #1173 links the dwell to PLC skip inputs.
• Alarms: Alarm P45 is triggered by incompatible G-code combinations like G28 or G53. Alarm P34 is triggered if G04 is executed while high-speed high-accuracy control modes (G05 P10000 or G05 P20000) are active.
• Versions: Lathe (L-series) systems support the U address, whereas Machining Center (M-series) systems restrict time and revolution commands to X and P. Multiple-Spindle Control II configurations disable the D address, dynamically tracking the PLC encoder instead.

Warning: Programming a revolution-based G04 dwell in G95 mode while the spindle is stopped (via M05) will cause the CNC system to wait indefinitely, locking up the machine until a manual override is initiated.

Brand Comparison

Comparison Topic	Fanuc	Siemens	Mitsubishi
Dwell Unit Execution	Seconds by default; Spindle Revolutions in G95 mode if Parameter 3405 bit 1 (DWL) is set to 1.	Seconds (G4 F...) or Spindle Revolutions (G4 S...) natively; adaptive to G94/G95 in ISO Dialect mode via MD20734 bit 2.	Seconds by default; Spindle Revolutions in G95 mode if Parameter #8130 is set to 1.
Address Formats	P (integer/ms dependent on Parameter 1020), X (seconds/decimal), U (lathe-only incremental).	F (seconds), S (master spindle revolutions), S<n>= (specific spindle), or X / P (ISO mode).	X (seconds/decimal), P (integer/scaled by factor), U (lathe-only incremental), and D (spindle selection).
Abort / Skip Dwell	Multi-stage skip Q-address inside G04 block immediately aborts dwell.	— (no source)	Dwell skip function directly configured by PLC input via parameter #1173 (dwlskp).
Secondary Spindle Dwell	— (no source)	Inline syntax G4 S<n>=... allows dwelling based on specific secondary spindle revolutions.	Multi-Spindle Revolution Dwell specifies spindle identifier D alongside G04 in G95 mode.
Timing Multiplier / Scaling	Locked to 1 ms via Parameter 1020 bit 7 (DWT) or depends on IS system.	— (no source)	Parameter #19014 scales integer P by a factor of 10<sup>-3</sup> to 10<sup>3</sup>.
Standalone Block Constraint	Cutter compensation active: consecutive G04 causes PS0041.	Must be programmed alone in block; other NC elements (synchronous actions/M-functions) cause Alarm 12120.	Numerical value must be placed after G04; combination with G28/G53 causes P45. Cannot dwell during G05 modes (triggers P34).

Technical Analysis

A deep technical analysis of these control systems reveals highly divergent philosophies in how dwell commands are integrated with the machine's hardware and PLC. Fanuc systems emphasize fine-grained parameter-level configurations, giving programmers explicit control over how the P address is scaled. By linking the DWT parameter (1020 bit 7) to either the active system increment (IS-B or IS-C) or locking it to a rigid millisecond scale, Fanuc provides maximum flexibility for multi-axis configurations but introduces programming ambiguity if decimal points are omitted. Furthermore, Fanuc uniquely allows G04 to interact directly with high-speed skip signals via the Q address, creating a hardware-level interrupt mechanism that is highly effective for rapid probing and skip cycles.

In contrast, Siemens operates on a structured, modular design that strictly separates G-code block functions while providing robust multi-spindle capability. Siemens natively allows the programmer to specify dwells in either seconds (F) or revolutions (S), and even target a secondary spindle using inline S<n>= syntax. This native multi-spindle support is completely distinct from the other brands, which must rely on parameter state changes or separate spindle identification addresses. However, Siemens enforces rigid syntactic isolation: programming any auxiliary command or G-function alongside G4 immediately triggers a syntax alarm (12120). Additionally, Siemens integrates G4 with its synchronized actions, requiring a dwell duration equal to at least two internal interpolator cycles (such as F0.1) to guarantee that non-modal PLC signals are successfully dispatched mid-program.

Mitsubishi blends these two paradigms by providing native multi-spindle address support while integrating a PLC-driven skip function that is entirely distinct from Fanuc's block-level skip signal. Mitsubishi's G04 skip condition is set directly via parameter #1173, mapping physical PLC inputs directly to the dwell execution. This allows the PLC to dynamically abort a dwell, whereas Fanuc's skip requires a dedicated Q address inside the NC block. Mitsubishi also utilizes a unique P factor parameter (#19014) to scale integer inputs by factors of 10^-3 to 10³. This powerful scaling mechanism is specifically designed to allow legacy code to run seamlessly across different machines without manual code modifications, resolving a major hurdle in multi-generation shop floors.

Program Examples

Fanuc Program Example

G94 G04 P1000 ; (Time-based dwell for 1.0 second under IS-B, or locks to 1ms dependent on Parameter 1020 DWT)
G95 G04 X30.0 ; (Dwell for 30 spindle revolutions when feed per revolution is active and Parameter 3405 DWL=1)
G04 X1.5 Q2 ;   (Dwell for 1.5 seconds, using multi-stage skip option assigned to skip signal Q2)

Fanuc Example Dry Run

In the first block, the G94 code sets feed per minute mode. The G04 P1000 command executes a dwell of exactly 1.0 second under the standard IS-B increment system (where 1 unit equals 1 millisecond), or locks strictly to 1 millisecond if parameter 1020 (DWT) is configured to 1, causing the dwell to finish prematurely. In the second block, the G95 code switches the machine to feed per revolution mode. With parameter 3405 (DWL) set to 1, G04 X30.0 instructs the controller to pause all axis interpolation until the spindle has completed exactly 30 full rotations. In the third block, the G04 X1.5 Q2 command pauses the axes for 1.5 seconds, but remains active to look for the high-speed skip signal assigned to skip selector Q2; if this PLC input signal triggers before the 1.5 seconds have elapsed, the dwell is immediately terminated and the control advances to the next program block.

Siemens Program Example

G04 F5 ;        (Pause execution for 5 seconds)
G4 S30 ;        (Dwell for 30 master spindle revolutions)
G4 S2=50 ;      (Dwell for 50 revolutions of secondary spindle 2)
G95 G04 X1000 ; (ISO Dialect Mode: Dwell for 1 spindle revolution when G95 is active and MD20734 bit 2 is set to 1)

Siemens Example Dry Run

In the first block, the G04 F5 command instructs the Siemens Sinumerik interpreter to pause all axis interpolation for exactly 5.0 seconds while the spindle continues to spin. In the second block, G4 S30 forces a dwell that is calculated based on spindle speed, pausing axis motion for exactly 30 rotations of the master spindle. In the third block, G4 S2=50 utilizes native multi-spindle capability, commanding a pause that lasts for exactly 50 revolutions of the secondary spindle (Spindle 2), which is crucial for synchronized sub-spindle part handoffs. In the fourth block, the system runs under ISO Dialect Mode (G291) with G95 active; the G04 X1000 command will dwell for 1 spindle revolution since MD20734 bit 2 is set to 1, which evaluates the input as spindle revolutions rather than seconds.

Mitsubishi Program Example

G94 G04 X5.0 ;  (Standard time-based dwell using the X address for 5.0 seconds in feed-per-minute mode)
G94 G04 P5000 ; (Time-based dwell using P address, subject to scaling parameter #19014 or validation parameter #8112)
G95 G04 X100. D1 ; (Revolution-based dwell for 100 revolutions synchronized against spindle 1 in G95 mode)

Mitsubishi Example Dry Run

In the first block, the G94 feed-per-minute mode is established, and G04 X5.0 pauses the tool axes for exactly 5.0 seconds. In the second block, G04 P5000 is commanded. If parameter #8112 (DECIMAL PNT-P) is set to 0, decimal points are ignored, and if scaling parameter #19014 is set to -3 (a 1/1000 multiplier), the 5000 integer value is scaled to 5 seconds. If #19014 is set to 0, it may dwell for 5000 milliseconds (5.0 seconds) or 5000 seconds depending on the system's base increment. In the third block, G95 feed per revolution mode is active; the G04 X100. D1 command instructs the machine to dwell for exactly 100 spindle revolutions synchronized directly against the encoder of Spindle 1, ensuring the tool pauses in sync with the physical spindle rotation.

Error Analysis

Brand	Alarm Code	Trigger Condition	Operator Symptom	Root Cause & Resolution
Fanuc	PS0041 (Interference in Cutter Compensation)	Commanding G04 consecutively with another non-movement block (like an auxiliary M-code) while G41 or G42 cutter compensation is active.	The machine stops moving and displays the PS0041 alarm on the screen, halting automatic execution.	The tool-path look-ahead vector is disrupted by consecutive non-movement blocks, leading to a calculated overcut. Avoid programming multiple dwell or non-movement blocks together when G41/G42 is active.
Fanuc	PS0370 (G31P/G04Q Error)	Programming a Q address value outside the valid range (1 to 4 for standard multi-stage skip, or 1 to 8 for continuous skip), or commanding Q on a system without the skip option.	Immediate program halt with a PS0370 alarm message before block execution.	An illegal Q value was commanded or the multi-stage skip option is not active on the control. Correct the Q address value or purchase/enable the skip function option.
Siemens	12120 (G function not separately programmed)	Programming auxiliary M-functions, synchronous actions, or other G-codes in the exact same NC block as the G4 dwell command.	The control rejects the block during execution, stops motion, and throws Siemens Alarm 12120.	Siemens requires that the G4 dwell command be programmed alone in a separate NC block. Move all auxiliary codes and synchronous actions to separate blocks.
Siemens	700013 (Operation not allowed: chuck unclamped)	Ignoring mechanical delays required for chuck clamping before executing tool movements.	The CNC safety system trips, interrupting the program and throwing Alarm 700013.	A movement block was commanded before the chuck's physical clamping mechanism had fully settled. Program a G4 dwell command to allow adequate time for the chuck clamp status to settle before movement.
Mitsubishi	P45 (G-Code Combination)	Commanding G04 in the exact same block as an incompatible G-code, such as G28 (Reference position return) or G53 (Machine coordinate system).	The machine halts immediately and displays the P45 alarm code, terminating active automatic cycle.	The NC parser encounters an illegal combination of a non-modal dwell and reference or coordinate setup codes. Program G04 in a standalone block or verify compatible G-code pairings.
Mitsubishi	P34 (High-speed high-accuracy control error)	Invoking a G04 dwell command while advanced modes like High-speed high-accuracy control II (G05 P10000) or III (G05 P20000) are active.	Cycle interruption and immediate display of the P34 alarm code on the controller screen.	Advanced path smoothing algorithms cannot process dwell pauses while actively active. Temporarily disable the G05 high-speed modes before executing any G04 commands.

Application Note

An infinite cycle hang will occur if a revolution-based dwell (G04) is commanded while the spindle is actively stopped (M05) in G95 mode under Mitsubishi controls with the '#8130 Dwell in rev.' parameter active. Because the machine is programmed to wait for a specific count of spindle revolutions, a stationary spindle prevents the encoder from registering rotation, trapping the control in an endless standby state that halts the entire production line. To prevent this, operators must ensure the spindle is actively rotating before executing a revolution-based dwell. Similarly, on Fanuc systems, an unexpected tool drag will occur if an integer P-value is programmed while parameter 1020 bit 7 (DWT) is set to 1, causing a programmed P1000 (intended as 1 second) to be interpreted as a mere 1 millisecond. This premature motion drags the tool across the workpiece before the cut is fully relieved, scraping the part. To eliminate mathematical ambiguity, programmers should utilize the X or U addresses with explicit decimals. Finally, on Siemens controls, a G4 command programmed alongside auxiliary M-codes will instantly trigger Alarm 12120, while neglecting hardware delays for clamping mechanisms will trigger Turret motor overload (Alarm 700022) or Tool clamping timeout (Alarm 700011). Programmers must strategically place standalone G4 blocks to let mechanical states settle, and avoid inserting G4 during smooth surfacing passes to prevent the tool from decelerating to a stop, which leaves visible witness marks on the finished surface.

Related Command Network

• G01 Linear Interpolation: G04 is frequently programmed between or at the end of G01 feed blocks to temporarily pause tool movement and relieve cutting pressure at the end of a linear pass.
• G02 Circular Interpolation: G04 can be used immediately after a G02 circular arc to allow tool pressure to settle and ensure a smooth, round finish on internal radii.
• G03 Circular Interpolation: Similar to G02, G04 provides a brief pause following a G03 counter-clockwise arc to allow the cutting forces to dissipate and prevent witness marks on workpiece corners.
• G09 Exact Stop: While G04 executes a timed pause, G09 is a non-modal code that forces the machine to decelerate to a complete stop at the end of a block to verify position before the next block begins.
• G31 Skip Function: The skip function allows axis movement to be terminated immediately by an external input signal, sharing similar PLC skipping logic with Mitsubishi's parameter-driven dwell skip.

Conclusion

Mastering the G04 dwell command requires aligning G-code syntax with the specific parameter configurations of Fanuc, Siemens, and Mitsubishi controllers. Programmers must verify active feedrate modes, confirm parameter-level scaling behavior, and ensure mechanical clamping delays are fully accommodated to prevent premature tool movements or severe syntax alarms. Implementing precise standalone dwell blocks is the key to maintaining tool-path integrity, protecting spindle and turret hardware, and achieving flawless surface finishes across all CNC machining operations.

FAQ

Why does my CNC machine wait infinitely when executing a revolution-based G04 dwell?

An infinite cycle hang occurs because the CNC is configured to count spindle rotations (such as in G95 feed-per-revolution mode with Parameter #8130 active on Mitsubishi, or Parameter 3405 active on Fanuc) while the spindle is physically stopped (via an M05 command). Since the spindle is stationary, the encoder registers zero revolutions, preventing the G04 block from satisfying its programmed count and stalling the program. To resolve this, always verify that the spindle is actively rotating before calling a revolution-based dwell, or program a modal feedrate switch to G94 (feed-per-minute) prior to the dwell block to force a time-based pause instead.

Why does my programmed P1000 dwell command execute for only a fraction of a second?

A microscopic dwell duration is caused by a parameter mismatch where the controller interprets the P address integer on a rigid millisecond scale instead of standard seconds. On Fanuc systems, if parameter 1020 bit 7 (DWT) is configured to 1, a value of P1000 is locked to exactly 1 millisecond (0.001 seconds), causing the machine to instantly resume axis movement. To ensure predictable dwells across all machine models, avoid the mathematical ambiguity of integer-only P commands and instead program your pauses using the X or U addresses with explicit decimal points (e.g., G04 X1.0) to guarantee a full one-second pause.

What causes a Siemens controller to throw Alarm 12120 when executing G4?

Siemens Sinumerik controls enforce a strict syntactic rule that requires the G4 dwell command to be programmed alone in a standalone NC block. If you attempt to program coolant codes (such as M08), spindle speed changes, or other G-codes (like G01 or G64) on the same line as G4, the block parser will immediately halt execution and trigger Alarm 12120. To eliminate this issue, isolate the G4 command completely by dedicating an entire line of code to the dwell (e.g., G4 F2.0) and positioning all auxiliary functions and path smoothing commands in the blocks directly preceding or following it.