How do you program the G81 drilling cycle on CNC machines Program the G81 drilling cycle by defining coordinates, depth Z, clearance R, and feedrate F. Under Fanuc systems, parameter 0001 bit 1 configures the format. If coordinates shift, cancel the modal cycle using G80 to prevent crashes and avoid triggering Alarm PS0206.
Introduction
Programmers and setup operators must maintain strict vigilance regarding coordinate zero offsets (such as G54) and active tool offset values before launching the canned cycle. Because tool compensations are ignored during the cycle's internal positioning calculations, any misalignment in the offset registers will shift the toolpath. Under these uncompensated conditions, the tool post turret or spindle head will travel along a dangerously shifted trajectory. The tool nose can bypass software boundaries and drive the rotating drill directly into physical barriers and workpiece workholding—shattering the tool against a raw stock vise jaw, table-mounted fixture clamps, or the rotating jaws of a spindle chuck. This positioning error results in a catastrophic hard collision (crash), shatters the drill, damages the spindle assembly, halts axis slides with an overload alarm code, and converts the expensive casting into a completely ruined scrap part.
Technical Summary
| Field / Parameter | Value / Specification |
|---|---|
| Command Code | G81, CYCLE81 (Siemens native mode) |
| Group / Modality | Group 09 (Fanuc / Mitsubishi / Siemens G291 ISO Dialect), Group 10 (Fanuc turning G-code list) |
| Supported Brands | Fanuc, Siemens, Mitsubishi |
| Critical Parameters | Fanuc Parameter No. 0001 Bit 1 (FCV), Siemens DP/DPR, Mitsubishi Parameter #1265 ext01/bit2 |
| Main Constraint | Rapid retraction straight from the hole bottom without dwelling makes G81 unsuitable for flat-bottom machining (use G82) or fine boring (retraction can scratch bore cylinder walls). |
Quick Read
- Select G81 for simple center drilling, chamfering, and spot drilling where a smooth bottom surface finish is not required.
- Verify that the clearance plane (Point R) height is set high enough to clear workholding jaws and raw stock.
- Toggle between G98 (return to initial plane) and G99 (return to R clearance plane) to control retraction behavior between holes.
- Deactivate G81 with a G80 cancel command before initiating coordinate transformations, tool changes, or axis switching.
- Ensure the spindle rotation direction (M03 or M04) is modally active before invoking the drilling cycle.
- Double-check parameters like Fanuc Parameter 5102#6 (RAB) to verify whether R-plane dimensions are parsed as incremental or absolute.
Basic Concepts of G81 Drilling
The practical programming effect of the G81 cycle on Fanuc systems is to optimize point-to-point drilling efficiency by consolidating positioning, rapid approach, feed, and retraction motions into a single block. Because G81 is a modal command, once it is programmed, the control retains the drilling parameters (such as the Point R level and Z-depth) and executes a complete drilling stroke at any subsequent coordinate block. This modal memory reduces program size, simplifies pattern programming, and keeps axis feed rates uniform when machining rows or grids of holes. Since G81 does not dwell at the bottom of the cut, it is utilized for shallow holes and center drilling where a smooth bottom surface finish is not required.
The practical programming effect of the G81 drilling cycle (or native CYCLE81) on Siemens SINUMERIK controls is to provide highly efficient, standardized centering and shallow hole drilling. By packaging axis positioning, rapid approach to safety planes, cutting feed to depth, and rapid retraction into a single parametric cycle, G81 reduces part program size and optimizes machining efficiency. The cycle is ideal for center drilling and chamfering operations because it executes rapid traverse retraction straight from the hole bottom without dwelling, reducing non-cutting time during high-volume production.
The practical programming effect of the G81 cycle on Mitsubishi systems is to consolidate multi-step positioning, safe-plane approaches, cutting feeds, and rapid retractions into a single, high-efficiency block. Because G81 is modal, the control retains the drilling parameters and automatically executes a drilling sequence at any subsequent coordinate block. This modal retention drastically reduces part program sizes and simplifies coordinate pattern programming. On turning centers equipped with live tooling, G81 utilizes active spindle clamping. When clamping is configured via Parameter #1183 clmp_M, the control automatically outputs the C-axis clamping M-code after initial positioning to lock the spindle. After retracting to the Point R safe clearance level, the unclamp command is output (clamp M-code + 1) and the tool dwells for the duration set in Parameter #1184 clmp_D before continuing to the next coordinates.
Command Structure and Syntax
The command syntax for G81 is structured to define the geometry and cutting feed rate in a single block. In standard ISO systems like Fanuc and Mitsubishi, coordinates are specified first, followed by Z-axis depth, R clearance height, and the cutting feedrate. When the compiler reads this block, it establishes these parameters modally. The machine will continue to perform this exact drilling sequence at every subsequent coordinate block until a cancellation code is programmed.
Siemens native programming uses the CYCLE81 format inside G290, which decouples the hole positions from the cycle definition. In Siemens mode, you define retraction and reference planes along with safety clearances as direct numerical inputs within the cycle parameters. For systems using the ISO dialect compiler (G291), the standard G81 syntax is parsed using traditional address characters.
Standard Syntax
; Fanuc / Siemens ISO Dialect / Mitsubishi Standard
G98 (or G99) G81 X_ Y_ Z_ R_ F_ K_ ;Siemens Native Syntax
CYCLE81 (RTP, RFP, SDIS, DP, DPR) ;Mitsubishi Special Syntax (Label L and Label O Formats)
G81 Xx1 Yy1 Zz1 Rr1 Ff1 LI1(Hh1), Ii1, Jj1 Dd1 Ee1 ;
G81 Xx1 Yy1 Zz1 Rr1 Ff1 Pp1, Ii1, Jj1 ;Active Parameters and Addresses
- X, Y (Center Coordinates): Absolute or incremental coordinates defining the hole center.
- Z (Final Drilling Depth): Absolute coordinate of the hole bottom or incremental distance from point R.
- R (Reference Plane / Point R): Height where tool transition shifts from rapid traverse to cutting feed.
- F (Cutting Feedrate): Machining feed rate programmed in mm/min or inch/min.
- K / L (Repeat Count): The number of times the drilling sequence is executed at incremental steps.
- RTP (Retraction Plane): Absolute Siemens retracted height position.
- RFP (Reference Plane): Absolute Siemens reference coordinate for workpiece zero surface.
- SDIS (Safety Clearance): Incremental Siemens clearance height added to the reference plane.
- DP (Absolute Depth): Absolute final drilling depth in Siemens coordinate system.
- DPR (Relative Depth): Incremental final drilling depth measured relative to reference plane.
Brand Applications: Fanuc, Siemens, and Mitsubishi
Fanuc
Fanuc systems manage G81 via modal group 09. Programmers configure the format check parameter, Parameter No. 0001 bit 1 (FCV), to toggle between standard Series 16 format and legacy Series 15 format, which shifts coordinate interpretation.
When G81 is active, the preprocessor executes the drill sequence using standard G-codes such as G90 for absolute coordinates and G91 for incremental movements.
| Configuration Element | Value / Code | Technical Behavior |
|---|---|---|
| System Parameter | Parameter No. 0001 Bit 1 (FCV) | Configures program format. 0: Standard, 1: Series 15 format. |
| System Parameter | Parameter No. 5102 Bit 3 (F16) | Format checking parameter for Series 15/16 format checking. If FCV=1: 0 for Series 15-T, 1 for Series 16. |
| System Parameter | Parameter No. 5102 Bit 6 (RAB) | Retraction plane coordinate interpretation in Series 15 format. 0: Incremental R, 1: Absolute G-code system A. |
| System Parameter | Parameter No. 1681 Bit 0 (DPS) | Positioning start-up block overlap capability. 0: Enabled, 1: Disabled. |
| System Parameter | Parameter No. 1681 Bit 1 (DRL) | Point R clearance boundary block overlap capability. 0: Enabled, 1: Disabled. |
| System Parameter | Parameter No. 1681 Bit 5 (DZL) | Bottom dwell point block overlap capability. 0: Enabled, 1: Disabled. |
| System Parameter | Parameter No. 5188 | Drilling count threshold to trigger cutting chip removal function. 0 or less disables. |
| System Alarm | Alarm PS0010 | IMPROPER G-CODE: Specified G-code does not exist or is unsupported. Check program syntax. |
| System Alarm | Alarm PS0206 | AXIS SWITCHING IN RIGID MODE: Switch active drilling axis without deactivating the cycle via G80. |
| System Alarm | Alarm PS0571 | PROGRAM MISS AT P-TAPPING: Tapping cycle commanded in Series 15 format without correct parameters. Set parameters PTE (12623#0) and PTX (12623#1). |
Siemens
Siemens controls execute drilling cycles through bimodal compilation. The channel-specific machine data MD 18800 $MN_MM_EXTERN_LANGUAGE enables the external ISO dialect compiler to parse standard G81 commands instead of native CYCLE81 calls.
In ISO mode (G291), G81 functions as a standard drilling cycle. In native mode (G290), CYCLE81 is invoked modally via MCALL, requiring separate coordinate declarations.
| Configuration Element | Value / Code | Technical Behavior |
|---|---|---|
| Cycle Parameter | RTP | Retraction plane absolute coordinate. Real value. |
| Cycle Parameter | RFP | Reference plane absolute coordinate. Real value. |
| Cycle Parameter | DP | Final drilling depth absolute coordinate. Real value. |
| Cycle Parameter | SDIS | Safety clearance. Positive incremental value. Real value > 0. |
| Cycle Parameter | DPR | Final drilling depth relative to reference plane. Positive incremental value. Real value > 0. |
| System Parameter | MD 18800 $MN_MM_EXTERN_LANGUAGE | Channel-specific machine data to enable external ISO dialect compiler. 1: Enabled. |
| System Alarm | Alarm 61101 | Reference plane defined incorrectly: RTP, RFP, or safety plane logically mismatched. |
| System Alarm | Alarm 61003 | No feed programmed in the cycle: Missing cutting feedrate F-word in cycle or modal registers. |
| System Alarm | Alarm 61102 | No spindle direction programmed: Missing M03 or M04 in modal registers. |
| System Alarm | Alarm 61815 | G40 not active: Tool radius compensation G41 or G42 active in ISO dialect mode. Deactivate before cycle. |
Mitsubishi
Mitsubishi systems utilize Parameter #1265 ext01/bit2 to toggle the MITSUBISHI CNC Special Format, allowing in-position checks to be defined inline. Spindle clamping during drilling cycles is governed by Parameter #1183 clmp_M.
Commanding G81 activates the drilling modal sequence, which can be modified using additional arguments such as ,I and ,J for in-position check widths.
| Configuration Element | Value / Code | Technical Behavior |
|---|---|---|
| System Parameter | Parameter #1265 ext01/bit2 | Switch for Mitsubishi CNC Special Format (enables special format address parsing like , I and , J). 0: Standard, 1: Special. |
| System Parameter | Parameter #19417 Hole deceleration check 2 | Deceleration check selection for the drilling axis. 0: No dec check, 1: Dec check, 2: Dec check at cut point + drive check sv024 at hole bottom. |
| System Parameter | Parameter #1271 ext07/bit1 | Toggles whether repetition command address Kk1 is enabled on control. 0: Disabled, 1: Enabled. |
| System Parameter | Parameter #1080 Dril_Z | Safety parameter that fixes active hole-drilling axis exclusively to Z-axis. |
| System Parameter | Parameter #1183 clmp_M | Defines C-axis clamping M-code. |
| System Parameter | Parameter #1184 clmp_D | Defines C-axis clamping dwell time. |
| System Alarm | Program Error (P411) | Axis Name Switching G111 commanded during an active G81/fixed cycle. Cancel cycle with G80 before commanding G111. |
| System Alarm | Program Error (P33) / (P128) | Machining Condition Selection command (G120.1/G121) issued during active drilling cycle. Cancel cycle with G80. |
| System Alarm | Program Error (P923) / (P261) | Coordinate rotations or 3D coordinate conversions (G68.1) commanded while G81 is active. Cancel G81 with G80 first. |
| System Alarm | Operation Error (M01 0107) | Calculated cutting speed and gear ratios exceed physical spindle clamp rate. Adjust programmed speed or spindle parameters. |
Brand Comparison
| Comparison Topic | Fanuc | Siemens | Mitsubishi |
|---|---|---|---|
| Cycle Activation | Canned cycle active from G81 command in same block as coordinates. | Activated with MCALL CYCLE81(...) (native) or G81 (ISO dialect). | Canned cycle active from G81 command in same block. Supports Special Format (,I and ,J). |
| Repeat / Repeat Count | Using K (Series 16) or L (Series 15) inside G81 block. | Hole locations and counts defined on separate lines or pitch circles; no repeat count inside cycle block in native mode. | Using LI (Label L) or Pp (Label O) or K based on Parameter #1271. |
| Axis Switching / Exchange | Switch axis after canceling canned cycle via G80. Switching inline triggers PS0206. | Managed by plane selections (G17/G18/G19) and technology cycles. | Change axis after canceling via G80. Inline switches trigger P411. |
Technical Analysis
Three distinct programmatic and preprocessor behaviors clearly distinguish Fanuc's coordinate and cycle handling from Siemens and Mitsubishi controls. First, Fanuc permits active canned cycles to be canceled on-the-fly using Group 01 motion commands. Under the Fanuc compiler, specifying a Group 01 motion command (such as G00 rapid traverse or G01 linear feed) in a subsequent block immediately cancels the active canned cycle, behaving exactly as if G80 had been commanded. Siemens native mode (G290) deactivates this behavior; modal cycles are called via MCALL and remain active across all coordinate blocks, ignoring G00 or G01 transitions until an explicit, standalone MCALL block is programmed.
Second, Fanuc manages repeat counts directly within the cycle block via a dedicated modal address. In Fanuc Series 16 format, the number of repetitions is commanded strictly using the K address, while Series 15 uses L. This contrast stands in opposition to native Siemens mode, where drilling positions are fully decoupled from G-code cycle blocks. Siemens utilizes the MCALL modal command to link a cycle block with a separate, coordinate-only subprogram or hole pattern macro (such as HOLES2 or CYCLE801), eliminating repeat count codes in the cycle block itself.
Third, Fanuc turning systems enforce list-dependent safety lockouts under active spatial transformations. If G81 is issued while simple inclined surface control (G176) or tool center point control (G174) is active, the preprocessor immediately blocks motion and triggers specialized program errors—such as P951/P942 or P952/P941 depending on the G-code list selection. Siemens and Mitsubishi controls manage coordinate frames on preprocessor stacks that do not enforce these exact multi-axis cycle conflicts natively.
In addition, Siemens incorporates G700 and G710 high-precision unit scaling. While standard Fanuc and Mitsubishi conversion G-codes (G20/G21 or G70/G71) only convert linear coordinate dimensions, Siemens extends this behavior through G700 and G710. These commands scale linear coordinate positions, active feedrates (F-values in mm/min vs. inch/min), and all length-related system variables dynamically, allowing seamless bilingual operations without manual calculation. Siemens also utilizes a toggled bimodal compiler (G290/G291) to define G81 cycle behavior. While Fanuc and Mitsubishi interpret G81 strictly as a standard, hardcoded drilling cycle, Siemens requires the programmer to explicitly toggle the interpreter to native Siemens mode via G290 to utilize CYCLE81. Toggling the compiler to ISO Dialect Mode via G291 deactivates native cycles, dynamically remapping G81 to an external G-code cycle.
Lastly, Mitsubishi controls utilize a dynamic bimodal Program Format Switch compiler (G188/G189) to translate drilling cycle tables on-the-fly. Commanding G188 switches the bimodal compiler from lathe format to machining center format. This action automatically cancels active lathe-specific canned cycles, initializes Group 24 registers, and reallocates G81 from an Electronic Gear Box (EGB) synchronization start command (Group 24 in turning lists) to a standard spot drilling cycle (Group 09). Fanuc and Siemens controls lack an integrated bimodal program format switch compiler of this kind, requiring distinct physical configurations and separate program streams. Mitsubishi also integrates a parameter-locked MITSUBISHI CNC Special Format (#1265 ext01/bit2 ON) that allows programmers to output positioning and drilling axis in-position widths directly inside the cycle block, and a dedicated parameter (#19417 Hole deceleration check 2) to selectively enforce deceleration checks or full in-position checks at the cut point and hole bottom during drilling cycles.
Program Examples and Dry Run Walkthroughs
Fanuc Spot Drilling and Tapping Canned Cycle Example
G90 G99 G81 X200.0 Y-150.0 Z-25.0 R3.0 F120.0 ;
G91 G98 G81 X-50.0 Y100.0 Z-30.0 R-5.0 F100.0 L3 ;
G80 G00 Z50.0 ;Dry Run Analysis: In block 1, the controller selects absolute coordinates (G90) and sets retract plane return (G99). G81 coordinates positioning to X200.0, Y-150.0. The spindle rapid-moves to the reference R-plane height of 3.0 mm. Axis feeds down to final depth Z-25.0 mm at 120.0 mm/min. The spindle rapid-retracts to the reference R-plane height (3.0 mm) after drilling is complete. In block 2, the controller switches to incremental positioning (G91) and initial plane return (G98). The tool moves X-50.0 mm, Y100.0 mm. G81 executes drilling to Z-30.0 mm relative to the current position, starting from the incremental R clearance plane of -5.0 mm at 100.0 mm/min. The tool retracts to the initial plane height (from before this block) instead of the R-plane. The loop count L3 (in Series 15 format compatible mode) repeats the drilling cycle 3 times, shifting the coordinates by the incremental step each iteration. In block 3, G80 cancels the active Group 09/10 modal canned cycle, clearing all Z-depth and R-plane clearance registers. The tool rapids to a safe clearance height of Z50.0.
Siemens Bimodal Native and ISO Mode Canned Cycle Example
G290 ;
MCALL CYCLE81 (110, 100, 2, 35) ;
X100.0 Y50.0 ;
X150.0 Y50.0 ;
MCALL ;Dry Run Analysis: In block 1, G290 switches the interpreter to native Siemens mode. In block 2, MCALL activates the CYCLE81 drilling cycle modally. The retraction plane is set to absolute 110 mm, the reference plane is set to 100 mm, safety clearance is 2 mm, and the absolute final depth is 35 mm. In block 3, the machine positions the axes to X100.0, Y50.0. Because MCALL is active, the preprocessor automatically executes the drilling cycle CYCLE81: rapid to the reference plane + safety clearance, drill to absolute depth Z35, and rapid-retract back to the retraction plane RTP (110 mm). In block 4, the machine positions to X150.0, Y50.0 and repeats the CYCLE81 drilling stroke. In block 5, the standalone MCALL statement cancels the modal cycle definition, returning the controller to standard linear programming mode.
Mitsubishi Fixed Cycle and Safety Lockout Example
G90 G99 G81 X100.0 Y-150.0 Z-25.0 R2.0 F150.0 LI1 ;
G188 G90 G99 G81 X50.0 Y50.0 Z-25.0 R2.0 F100.0 ;
G80 G00 Z50.0 ;Dry Run Analysis: In block 1, in absolute coordinates (G90), the machine rapids to coordinates X100.0, Y-150.0 and prepares the G81 canned cycle. The tool rapid-moves to the R-plane height of 2.0 mm, feeds down to Z-25.0 mm at 150.0 mm/min, and rapid-retracts to the R-plane in G99 mode. LI1 dictates that the cycle is executed once (repeat count of 1). In block 2, G188 activates the program format switch compiler, resetting Group 09. The machine selects G90 and G99 and initializes a new G81 cycle at coordinates X50.0, Y50.0. The tool rapid-moves to the R-plane of 2.0 mm, feeds down to depth Z-25.0 mm at 100.0 mm/min, and retracts to R-plane. In block 3, G80 cancels the active Group 09 modal drilling cycle, clearing all Z-depth and R-plane registers. G00 rapids the tool to Z50.0.
Error Analysis
| Brand | Alarm Code | Trigger Condition | Operator Symptom | Root Cause / Fix |
|---|---|---|---|---|
| Fanuc | Alarm PS0206 | Switch active drilling axis without deactivating the cycle via G80. | The machine axis halts immediately mid-program with a red alarm light flashing. | Cancel drilling cycle via G80 before changing drilling axis. |
| Fanuc | Alarm PS0010 | Specified G-code does not exist or is unsupported. | Program execution halts at the erroneous G-code block. | Check program syntax and active options. |
| Fanuc | Alarm PS0571 | Tapping cycle commanded in Series 15 format without correct parameters. | Tapping cycle commanded in Series 15 format fails to run. | Set parameters PTE (12623#0) and PTX (12623#1). |
| Siemens | Alarm 61101 | RTP, RFP, or safety plane logically mismatched. | The control panel displays Alarm 61101, halting cycle compilation. | Ensure retraction plane and reference plane coordinates are logically sequential. |
| Siemens | Alarm 61003 | Missing cutting feedrate F-word in cycle or modal registers. | The cycle halts immediately after positioning, before plunging. | Program feedrate F-word before calling cycle. |
| Siemens | Alarm 61102 | Missing M03 or M04 in modal registers. | The machine axis moves to coordinates but refuses to feed down. | Program M03 or M04 spindle start before calling cycle. |
| Siemens | Alarm 61815 | Tool radius compensation G41 or G42 active in ISO dialect mode. | The cycle is aborted before any coordinate positioning occurs. | Ensure tool radius compensation is deactivated with G40 before cycle. |
| Mitsubishi | Program Error (P411) | Axis Name Switching G111 commanded during an active G81/fixed cycle. | The screen displays Program Error (P411), and execution is aborted. | Cancel cycle with G80 before commanding G111. |
| Mitsubishi | Program Error (P33) / (P128) | Machining Condition Selection command (G120.1/G121) issued during active drilling cycle. | The NC shuts down axis motion with program error codes. | Cancel cycle with G80 before condition selection. |
| Mitsubishi | Program Error (P923) / (P261) | Coordinate rotations or 3D coordinate conversions (G68.1) commanded while G81 is active. | The preprocessor flags the conversion command as illegal. | Cancel G81 with G80 before coordinate transformations. |
| Mitsubishi | Operation Error (M01 0107) | Calculated cutting speed and gear ratios exceed physical spindle clamp rate. | Spindle clamping fails to complete, throwing an operation error. | Adjust programmed speed or spindle parameters. |
Application Notes: Advanced Drilling Safety
A catastrophic spindle crash and shattered tooling will occur if coordinate zero offsets (such as G54) and active tool length offset registers are misaligned before launching the canned cycle. Because tool compensations are ignored during the internal positioning calculations of G81, the tool post turret or spindle head will travel along a dangerously shifted trajectory. The rotating drill nose will bypass software boundaries and drive directly into physical barriers and workpiece workholding. This positioning error shatters the tool against a raw stock vise jaw, table-mounted fixture clamps, or the rotating jaws of a spindle chuck. To prevent this positioning error, setup operators must dry-run newly generated programs in single-block mode and verify safety clearances on the HMI coordinate screen before enabling high-speed automatic execution.
Related Command Network
- G80: Cancels active drilling cycle modal states and flushes depth and clearance registers. View the detailed guide on G80 Canned Cycle Cancel.
- G82: Drilling cycle with dwell, used for spot drilling when a flat-bottom surface finish is required.
- G83: Deep-hole peck drilling cycle, used when cutting chips must be evacuated to prevent drill breakage. Learn more about peck drilling in the G73 High-Speed Peck Drilling Cycle.
- MCALL: Native Siemens modal call command, used to bind CYCLE81 to coordinate lists.
- G60: Single direction positioning command used to eliminate backlash. Learn more about this at the G60 Single Direction Positioning Guide.
Conclusion
Success in canned cycle programming depends on maintaining absolute synchronization between the CNC preprocessor's modal memory and the physical state of the machine. Operators must verify zero coordinate offsets and cancel active G81 cycles using G80 before applying any spatial transformations or tool changes. Consistently implementing these practices on the shop floor eliminates uncompensated movements, minimizes setup alarms, and prevents expensive collisions.
Frequently Asked Questions
Why does G81 ignore cutter radius compensation during execution?
Canned cycles like G81 calculate positioning trajectories along the center axis of the tool, rendering tool radius offsets (G41/G42) inactive during execution. If radius compensation remains active, the preprocessor may output path deviations or trigger Alarm 61815. Always deactivate cutter compensation with G40 before commanding G81, and verify on the control screen that the offset coordinates are zeroed.
How does Parameter No. 0001 (FCV) affect Fanuc G81 repetition programming?
This parameter determines whether the Fanuc interpreter uses standard Series 16 format or legacy Series 15 format. When FCV is set to 1, the repetition count address shifts from K to L, and the R-plane coordinate can be parsed as absolute. Programmers must check the active controller model and verify parameter settings on the HMI screen before translating programs to prevent syntax errors.
What is the benefit of using Parameter #19417 on Mitsubishi G81 cycles?
Parameter #19417 allows programmers to select the deceleration check behavior at the hole bottom. Configuring this parameter to 2 enables a deceleration check at the cut point and a drive check sv024 at the hole bottom, preventing axis lag from dragging the tool or scratching the surface. Shop operators should configure this parameter to optimize hole bottom consistency during high-speed production runs.