G98 and G99 Cycle Return Levels: Complete CNC Programming Guide

Introduction

A rapid lateral traverse at the wrong elevation can instantly drive a carbide drill into a heavy steel clamp, a workholding vise jaw, or a rotating spindle chuck, causing a high-impact mechanical collision. When this happens, the operator sees a sudden axis overload, hears a loud crash, and is forced to press the emergency stop as the machine displays an alarm code. The tool breaks, the workpiece is scrapped, and the spindle alignment is ruined, requiring costly maintenance and downtime. This catastrophic sequence is a direct consequence of leaving the G99 R-plane return mode active when the retraction plane is set below the height of physical obstacles on the workpiece.

Understanding the difference between G98 and G99 commands prevents these errors. In canned cycles, G98 returns the tool to the initial starting plane, while G99 returns it to the R-point clearance plane. Selecting the wrong code represents one of the most common programming mistakes on the shop floor. To learn about absolute coordinate systems, refer to the G90 and G91 Absolute vs. Incremental Programming guide.

Technical Summary

Technical Specification	Details
Command Codes	G98 (Initial Plane Return / Feed per Minute), G99 (R-Plane Return / Feed per Revolution)
Modal Group	Group 10 (Canned Cycle Retract on Fanuc), Group 11 (Siemens ISO Dialect), Group 05 (Lathe Feedrate on Fanuc/Mitsubishi System A)
Supported Brands	Fanuc, Siemens, Mitsubishi
Critical Parameters	Parameter 3401 bit 1 (FCD), Parameter 3402 bit 4 (FPM), Global User Data _ZFPR[6], Parameter #8013
Main Constraint	Must cancel active tool radius compensation (G40) before cycle call; G98/G99 functions overload on lathes depending on active G-code system lists.

Quick Read

• Assess clearances first: Select G98 to retract the tool fully to the initial starting plane when traversing over tall clamps, ribs, or fixtures.
• Minimize cycle times safely: Program G99 to retract the tool to the lower R-plane clearance height when drilling multiple holes on flat, unobstructed surfaces.
• Verify G-code system layout: Check if your turning control operates on Lathe System A, where G98 and G99 act as feedrate mode controllers rather than cycle retract levels.
• Cancel tool nose compensation: Always program G40 before calling a canned cycle block to avoid triggering a P155 program error.
• Inspect stroke limits: Ensure the calculated tool path end point does not enter a prohibited area, which immediately triggers a P452 alarm on Mitsubishi.
• Handle feedrate mode switches: Program the feedrate (F) value explicitly in the same block after switching between feed-per-minute (G98) and feed-per-revolution (G99) on lathes to prevent feed-zero alarms like Fanuc PS0011.

Basic Concepts

Hole-making operations utilize canned cycles to automate repetitive machining actions such as drilling, boring, and tapping. To manage the tool's retraction between these consecutive hole locations, programmers use G98 and G99 commands. These commands are modal, meaning the selected retraction level remains in effect for all subsequent operations until the alternative code is commanded.

When a canned cycle is executed, the tool operates between three distinct Z-axis planes. The first is the initial starting plane, which is the absolute Z-axis coordinate where the tool was positioned immediately before the cycle was first invoked. The second is the retraction plane (point R), which is a coordinate set slightly above the workpiece surface. The third is the final hole depth. G98 forces the tool to retract completely to the initial plane between holes, providing maximum clearance. G99 commands the tool to retract only to the R-plane, keeping the tool close to the workpiece surface and minimizing rapid traverse time in open air.

Command Structure

A canned cycle block is structured to define coordinates, depths, feedrates, and retract behavior in a single line of G-code. The choice between G98 and G99 is modal and dictates the tool's path after completing the machining operation at the bottom of a hole. When G98 is active, the tool retracts rapidly to the initial plane before moving to the next hole coordinate. When G99 is active, the tool retracts only to the R-plane clearance height, then performs the lateral traverse.

The command block structure combines the return level, the canned cycle code, hole coordinates, depth coordinates, clearance planes, and feed values. The programming syntax defines the relationship between these variables. The controller parses these codes to determine the speed and direction of the axes.

Syntax Structure:

G98 G81 X[coordinate] Y[coordinate] Z[depth] R[plane] F[feedrate] ; Initial Plane Return
G99 G81 X[coordinate] Y[coordinate] Z[depth] R[plane] F[feedrate] ; R-Plane Return

Parameters & Addresses:

• G98: Modal command selecting retraction to the initial Z-axis start plane. On Lathe System A, it selects Feed per Minute (mm/min or inch/min).
• G99: Modal command selecting retraction to the point R clearance plane. On Lathe System A, it selects Feed per Revolution (mm/rev or inch/rev).
• X / Y: Hole center coordinates on the active working plane.
• Z: Absolute coordinate of the bottom of the hole, or the incremental distance from the R-plane.
• R: Absolute coordinate of the retraction plane (clearance height), or incremental distance from the start plane.
• F: feedrate value, which is interpreted as mm/min under G98 (lathe feed) or mm/rev under G99 (lathe feed). These lathe velocity modes are closely related to the G94 and G95 Feed Rate Modes used in milling and turning operations.

Brand Applications

Fanuc

Fanuc CNC controls utilize specific system parameters to govern how the interpreter processes G98 and G99. Parameter 3401 (bit 1, FCD) determines whether an F-code programmed before a G98/G99 feedrate switch adopts the new mode or inherits the old state. Additionally, parameter 3402 (bit 4, FPM) dictates the default modal feedrate state on system power-up.

The Fanuc G-code syntax varies between milling (M-series) and turning (T-series). For milling, canned cycles like G81 and G83 integrate G98 and G99 to control the return height. For lathes operating on G-code System A, G98 and G99 are mapped directly to feedrate velocity modes.

Category	System Setting / Code	Description / Behavior
Parameters	Parameter 3401 bit 1 (FCD)	Determines if an F-code physically programmed before a G98/G99 feedrate command in the same block inherits the old mode (0) or adopts the new one (1).
Parameters	Parameter 3402 bit 4 (FPM)	Dictates default modal feedrate state on system power-up/reset. 0 = G99 (feed/rev), 1 = G98 (feed/min).
Parameters	Parameter 0036 bit 4 (G98)	Power-up feed mode specifically for 0-GCD grinding series. 0 = feed per revolution, 1 = feed per minute.
Alarms	PS0010	Improper G-code. Triggered if G98/G99 is programmed but machine lacks the corresponding option, or in an improper state.
Alarms	PS0011	Feed zero command. Triggered on T-series if an axis command is executed without specifying a feedrate immediately after switching G98/G99 modes.
Versions	M-Series vs. T-Series System A	Milling controls use G98/G99 for canned cycle retract levels. Lathes using standard G-code System A map G98/G99 strictly to feedrate mode (feed/min vs. feed/rev). Switching lathe parameters to G-code System B or C restores cycle retraction behaviors for G98/G99.

Failure to clear turret and chuck boundaries when executing G99 canned cycles can cause mechanical crashes. In systems where C-axis clamps are integrated, executing a retract command while a clamp is engaged will result in a tool collision. Operators must monitor feedrate transitions on System A lathes to avoid dangerous tool acceleration.

Siemens

In Siemens controls operating in ISO Dialect mode, cycle return heights are processed natively within the system's global variables. The interpreter maps the active retraction position directly to the Global User Data (GUD) array parameter _ZFPR[6]. This setting dictates whether Siemens' internal shell cycles process legacy ISO code as G98 or G99.

Siemens controls execute canned cycles such as G82 and G89 with G98 and G99 return modes. When G98 is programmed, the tool returns to the initial starting plane; when G99 is active, the tool retracts only to the programmed reference plane.

Category	System Setting / Code	Description / Behavior
Parameters	_ZFPR[6]	Global User Data (GUD) array parameter used internally to store the active ISO dialect retraction level. Value of 1 represents G98, and 2 represents G99.
Parameters	R address	Specifies the retraction plane height. Can be an absolute coordinate or incremental distance from the starting plane.
Parameters	Z address	Specifies the final hole depth. Can be an absolute coordinate or incremental depth from the retraction plane.
Alarms	Alarm 61101	Reference plane defined incorrectly. Triggered if the retraction plane (R-plane) is improperly defined relative to the start plane or final Z depth, creating a geometric conflict.
Alarms	Alarm 61808	Final drilling depth or single drilling depth is missing. Triggered if the total depth Z or single pecking depth Q is completely omitted in the initial block.
Versions	G-code System A vs. B/C	System A implicitly forces tool return to the initial starting plane (G98 behavior). System B and C allow full modal differentiation between G98 and G99.

Programmers must ensure that active protection zones are fully cleared when leaving G99 active near fixtures. Setting the retraction plane lower than a physical clamping axis or double turret can trigger an immediate protection zone violation or cause a hard collision.

Mitsubishi

Mitsubishi CNC systems process canned cycles through a highly isolated modal architecture that protects the main program's active coordinate system. The control adjusts fixed cycle acceleration profiles using parameter #1253 (set25/bit2). Additionally, parameter #8013 determines the specific retract amount used in deep hole drilling cycles.

The G-code syntax on Mitsubishi utilizes G98 for initial point level return and G99 for R-point level return. Canned cycles such as G83 and G73 execute these modal commands to manage axis retracts. On Lathe lists 2, 4, and 6, G98 and G99 are remapped to feedrate velocity modes.

Category	System Setting / Code	Description / Behavior
Parameters	Parameter #1253 set25/bit2	Acceleration/Deceleration mode change in hole drilling cycle. If set to 1, cycle time may increase when the feedrate override is less than 100%.
Parameters	Parameter #8013	Specifies the retract or return amount ("m") in deep hole drilling (G83) or stepping (G73) cycles. Valid range is 0 to 199999998 (0.5µm units).
Parameters	Parameter #1566	Determines whether rapid traverse escape and return within fixed cycles conform to rapid feedrate parameter #2001.
Alarms	P155	Program error. Triggered when a fixed drilling cycle is called while tool nose R compensation (G41 or G42) is active.
Alarms	P452	Program error. Triggered if a travel path within a fixed cycle block attempts to move the tool into a stored stroke limit prohibited area.
Alarms	P186	Program error. Spindle command (S) is improperly issued while Punchtap cycle modal is active.
Versions	Lathe Lists 2, 4, 6	Fixed cycle initial return level is locked. G98/G99 cannot be used for cycle retract level toggles; they serve strictly as feedrate mode controllers (G98 = feed/min, G99 = feed/rev).

Prior to initiating a cycle return command, operators must cancel all tool radius compensations with G40 to prevent immediate program termination. Programmers must also utilize the G22 chuck barrier check function to prevent the tool nose from colliding with the chuck or tailstock due to depth programming errors.

Brand Comparison

Topic / Feature	Fanuc	Siemens	Mitsubishi
Native Cycle Returns	G98 (Initial plane) and G99 (R-plane) are modal retraction levels in canned cycles (Group 10).	ISO Dialect G98/G99 maps to group 11 modal commands in fixed drilling cycles.	G98 (Initial point return) and G99 (R point return) are modal return level commands.
Lathe System Overloads	Overloads G98/G99 as feedrate modes (feed/min vs. feed/rev) under standard System A.	System A locks out G99 behaviors and implicitly forces return to starting plane (G98).	Lock retract toggles on G-code lists 2, 4, 6 and remaps G98/G99 strictly to feedrate modes.
Internals & Extensibility	Highly micro-controlled via parameters such as 3401 (FCD) and 3402 (FPM) to dictate power-up/clear state and F-code inheritance.	Translates G98/G99 modal levels directly into Global User Data (GUD) parameter _ZFPR[6] (1=G98, 2=G99).	Isolates fixed cycle modals from main program via dedicated internal G.1 commands, preserving WCS state.
Safety & Boundaries	Restricts canned cycle motion based on chuck barrier parameters and turret boundary parameters.	Active protection zone violation controls can abort lateral traverse if R-plane is too low.	Pre-evaluates internal travel paths; throws P452 alarm code instantly if endpoint enters stroke limit prohibited area.

Technical Analysis

Comparing the architectural implementations reveals how each control handles coordinate processing and modal states. Fanuc relies heavily on parameter-driven micro-controls, allowing the machine builder to customize the G-code environment. For instance, the transition between feedrate modes on a Fanuc lathe is governed by parameter 3401 bit 1 (FCD). This allows the system to determine whether an F-code placed before a G98/G99 command in the exact same block inherits the old modal state or cleanly adopts the new one, preventing dangerous feedrate assumptions during complex coordinate shifts. These feed rate settings are often combined with constant spindle speeds or surface speeds like G96 and G97 Constant Surface Speed and Constant RPM.

In contrast, Siemens translates legacy ISO G98 and G99 return commands directly into its native Global User Data (GUD) architecture. The interpreter passes the active retraction state straight into the system variable _ZFPR[6], mapping G98 to a value of 1 and G99 to a value of 2. This direct translation allows Siemens' own advanced internal shell cycles to process legacy ISO code without requiring secondary post-processor modifications. It also allows the controller to enforce G-code system dependencies, locking out G99 behaviors in System A while granting full G98/G99 differentiation in Systems B and C.

Mitsubishi distinguishes itself by isolating the fixed cycle's internal modals from the main program. It utilizes a dedicated internal G.1 command to execute the fixed cycle operation, meaning the cycle uses its own group 01 modal information. When the cycle completes, the active modal is automatically restored to G00, eliminating the need for the programmer to manually restate the movement modal. Furthermore, Mitsubishi pre-evaluates the internal operations of the cycle block rather than waiting for physical travel. If a calculated coordinate path enters a prohibited stored stroke limit area, the control immediately throws a P452 alarm code and halts before any physical axis movement occurs.

Program Examples

Fanuc G-Code Example

G90 G99 G83 X100.0 Y50.0 Z-30.0 R5.0 Q8.0 F120.0 ;
X150.0 Y50.0 ;
G98 X200.0 Y100.0 Z-30.0 R5.0 Q8.0 ;

Dry Run Breakdown

• Block 1: The tool moves at rapid traverse to the initial plane (Z50.0) before the cycle starts. The coordinate mode is absolute (G90). G99 is activated, meaning the tool retracts only to the R-plane after drilling. G83 initiates a deep-hole peck drilling cycle at X100.0 Y50.0, drilling to a final depth of Z-30.0 with a peck depth (Q) of 8.0 mm and a feedrate (F) of 120.0 mm/min. The R-plane (R5.0) sets the starting clearance coordinate. After the hole is drilled, the tool retracts to Z5.0 (R-plane) and remains there.
• Block 2: The tool traverses laterally at rapid feed to X150.0 Y50.0 at the R-plane elevation (Z5.0). The peck drilling cycle repeats. Upon completion, the tool retracts again to Z5.0 (R-plane).
• Block 3: G98 is commanded, changing the modal retract level to the initial plane. The tool traverses to X200.0 Y100.0 and executes the peck drilling cycle. After reaching the Z-30.0 depth, the tool retracts all the way to the initial starting plane (Z50.0), clearing any physical fixtures.

Siemens G-Code Example

G90 G99 G82 X300.0 Y-250.0 Z-150.0 R-100.0 P1000 F120 ;
X400.0 ;
G98 Y-350.0 ;

Dry Run Breakdown

• Block 1: The control operates in absolute mode (G90). G99 is activated, establishing that retraction will occur to the reference plane. The G82 drilling cycle with dwell is called at coordinates X300.0 Y-250.0. The tool drills to the final depth of Z-150.0, starting from the reference plane (R-100.0), with a dwell time (P) of 1000 milliseconds at the bottom of the hole and a feedrate of 120 mm/min. The retraction height is mapped to _ZFPR[6] = 2 (G99). The tool retracts to the reference plane coordinate (Z-100.0).
• Block 2: The tool moves at rapid traverse to X400.0 Y-250.0, keeping the Z-axis at Z-100.0 (reference plane). The G82 cycle repeats. The tool retracts to Z-100.0.
• Block 3: G98 is activated, changing _ZFPR[6] to 1. The tool traverses to Y-350.0 and executes the G82 cycle. Upon reaching the Z-150.0 depth and completing the dwell, the tool retracts fully to the initial starting plane coordinate.

Mitsubishi G-Code Example

G90 G98 G83 X100.0 Y100.0 Z-50.0 R25.0 Q10.0 F1000 ;
G99 G73 X200.0 Z-50.0 R25.0 Q10.0 F1000 ;

Dry Run Breakdown

• Block 1: The controller is placed in absolute programming (G90). G98 is commanded, selecting initial point level return. The G83 deep-hole drilling cycle is called at X100.0 Y100.0. The tool rapid traverses to the initial starting plane (Z50.0), then feeds down to Z-50.0 in pecks (Q) of 10.0 mm starting from the R-plane clearance level of Z25.0. Upon completion of the hole, the tool retracts all the way up to the initial Z-axis start point (Z50.0).
• Block 2: G99 is commanded, switching the modal retract level to the R-point clearance plane. G73 initiates a step drilling cycle at X200.0 Y100.0 (inheriting Y). The tool rapid traverses at the initial plane to the new coordinates, feeds down to Z-50.0 with 10.0 mm pecks, and retracts only to the R-plane coordinate (Z25.0) after finishing, saving rapid traverse movement time.

Error Analysis

Brand	Alarm Code	Trigger Condition	Operator Symptom	Root Cause / Fix
Fanuc	PS0010	Programming G98 or G99 when the canned cycle option is missing or in an improper coordinate state.	The CNC control halts execution and displays the error message "PS0010 IMPROPER G-CODE". The red alarm light illuminates.	Verify that the machine parameters support the canned cycle option and check that the G-code system is in a valid state.
Fanuc	PS0011	Executing an axis move after switching between G98 and G99 on a T-series lathe without defining a feedrate.	The tool stops immediately, feed motion is halted, and the controller displays "PS0011 FEED ZERO COMMAND".	Program an explicit F-value (feedrate) immediately in the same block after switching feedrate modes.
Siemens	Alarm 61101	Defining the reference plane (R-plane) geometrically lower than the final Z depth or higher than the start plane.	The controller immediately aborts the active cycle block and displays "Alarm 61101 Reference plane defined incorrectly".	Correct the coordinates of the reference plane R or adjust the total Z depth values to ensure a logical tool path.
Siemens	Alarm 61808	Omiting the required total depth Z or the single peck depth Q in the first cycle block.	The tool remains stationary, and the control halts with the error message "Alarm 61808 Final drilling depth or single drilling depth is missing".	Program the Z coordinate or Q pecking parameter explicitly inside the first cycle command block.
Mitsubishi	P155	Commanding a fixed drilling cycle while tool nose radius compensation (G41 or G42) is active.	The CNC program halts immediately, displays "P155 Program error", and prevents the tool from executing the canned cycle.	Add a G40 command to cancel cutter radius compensation prior to invoking any fixed drilling cycles.
Mitsubishi	P452	A travel path within a fixed cycle block attempts to move the tool into a stored stroke limit prohibited area.	The axes immediately stop before physical traverse begins, and the CNC displays the error "P452 Program error".	Verify clearance heights and work coordinate boundaries to ensure the coordinates do not cross the software stroke limits.
Mitsubishi	P186	Issuing an spindle command (S) during a Punchtap cycle modal.	The controller throws "P186 Program error" and aborts the tapping operation.	Eliminate conflicting S-codes from the program or deactivate the Punchtap cycle before commanding a spindle speed.

Application Note

A catastrophic crash occurs when a programmer commands a G99 R-point level return but fails to realize the R-plane is set geometrically lower than a physical workholding fixture. When executing the cycle, the tool does not retract to the initial Z-plane between holes, and instead traverses laterally at the lower elevation. The indexing turret moves at rapid traverse, forcing the carbide drill directly into a fixture clamp, a workholding vise jaw, or the rotating spindle chuck. The operator sees a high-impact collision, hears a loud impact, and must immediately press the emergency stop as the machine displays an alarm. The tool breaks, the workpiece is scrapped, and the spindle alignment is ruined, requiring thousands of dollars in repairs and days of lost production.

To establish safe cycle return states, programmers must meticulously verify coordinate boundaries and obstacle heights before executing a program. For machining centers, G98 forces the tool to retract completely to the initial starting plane, guaranteeing safe clearance over tall fixtures. On Lathe controls, operators must establish clear parameter settings, using the G22 chuck barrier check function to prevent the tool nose from entering prohibited regions. Prior to cycle call, always cancel active tool radius compensation (G41/G42) using G40 to prevent P155 program errors.

Related Command Network

• G80 (Canned Cycle Cancel): Terminates the active canned cycle modal, restoring the machine to standard linear interpolation modes and preventing unwanted hole-making cycles.
• G81–G89 (Canned/Fixed Cycles): A family of modal commands for automated drilling, boring, and tapping that rely on G98 and G99 to determine their retraction heights.
• G94 / G95 (Feedrate Modes): Toggles the cutting feed speed between feed per minute and feed per revolution, which corresponds to the secondary function of G98 and G99 on lathe systems.
• G90 / G91 (Absolute vs. Incremental Positioning): Governs whether coordinate movements and retraction heights are processed as absolute positions or incremental distances.
• G22 (Chuck/Fixture Barrier Boundary Check): Establishes software boundaries that prevent the tool nose from colliding with the chuck or tailstock during cycle execution.

Conclusion

Managing canned cycle retraction levels is a fundamental skill that directly impacts both cycle efficiency and machine safety. Programmers must develop a habit of inspecting every hole-making pattern for tall clamps or fixture components that rise above the retraction plane. By default, coding G98 at the start of a pattern ensures the tool clears all obstacles, while strategically applying G99 on flat, open faces minimizes non-cutting rapid traverse motion. Combining this spatial awareness with strict parameter verification guarantees high-quality, collision-free CNC operations.

Frequently Asked Questions

What is the primary difference between G98 and G99 in a canned cycle?

G98 forces the tool to retract completely to the initial starting plane—the Z-coordinate where the tool was positioned immediately before the cycle was called—while G99 retracts the tool only to the R-plane clearance height. Programmers should select G98 whenever the tool must clear clamps or high features, and use G99 only on flat, open surfaces to reduce cycle times. Before executing a program, dry-run the toolpath on the CNC's graphic trace screen to confirm that retraction movements match the workpiece topography.

Why does G99 cause a collision with a workholding vise jaw or fixture clamp?

G99 commands a lateral rapid traverse between holes at the lower retraction plane coordinate rather than returning to the initial starting plane. If the R-plane height is set below the physical height of a vise jaw, fixture clamp, or workholding hardware, the tool will travel directly through the obstacle, causing a high-impact crash. Programmers must physically measure the highest point of the workholding setup and ensure that either the R-plane is set above this height or that G98 is explicitly programmed to retract the tool safely over the clamps.

Can G98 and G99 control both canned cycle retracts and lathe feedrates?

Yes, G98 and G99 have a dual identity that is determined entirely by the active G-code system and machine configuration. While machining centers use G98 and G99 to control canned cycle retraction levels, lathes using standard G-code System A map G98 and G99 strictly to feedrate velocity modes, where G98 commands feed-per-minute and G99 commands feed-per-revolution. CNC operators must verify their control's active parameter configuration and G-code system lists before programming to prevent inadvertently changing lathe feed speeds when attempting to control clearance heights.