What is the G83 deep-hole peck drilling cycle on CNC machines The G83 deep-hole peck drilling cycle automates deep axial drilling by periodically retracting the tool to clear chips. Standard cycles retract to Point R clearance level, while high-speed cycles retract by clearance distance d, managed by Parameter 5115 or VARI, to prevent tool breakage and Alarm 61101.
Deep-Hole Peck Drilling Failure Risks
When executing deep axial drilling on CNC machines, programming errors or coordinate offset shifts quickly escalate into severe tool and spindle damage. A critical failure scenario occurs when the in-position check width for retraction is configured too large relative to the physical safety distance from the Point R level to the workpiece face. In this condition, the controller registers completion of the retraction stroke prematurely and commands a rapid traverse stepover to the next coordinate before the drill flutes have cleared the top of the hole. The resulting lateral trajectory deviation drives the indexing turret or spindle head directly into workholding fixtures—such as a raw stock vise jaw, table-mounted clamps, or rotating spindle chuck jaws. This hard collision shatters the solid carbide or indexable drill, bends axis ball screws, halts axis travel with high-current servo overload alarms, and converts the expensive casting into a scrapped part.
G83 Technical Summary
| Technical Detail | Specification |
|---|---|
| Command Code | G83 (Fanuc, Mitsubishi, Siemens ISO Dialect), CYCLE83 (Siemens Native) |
| Modal Group | Group 09 (Fanuc, Mitsubishi), Group 10 (Siemens G291), Modally active (Siemens CYCLE83) |
| Supported Brands | Fanuc, Siemens, Mitsubishi |
| Critical Parameters | Peck Depth (Q or Qq), Retraction Clearance (Parameter 5115 / #8013 / _VRT), Degression Factor (DAM) |
| Main Constraint | Must be canceled with a G80 or empty MCALL block before subsequent coordinates or coordinate transformations. |
Quick Read: G83 Key Takeaways
- Evacuate Chips Safely: Select G83 deep-hole peck drilling to periodically retract the drill out of the hole, preventing flute packing, excessive friction, and thermal failure.
- Workholding Alignment: Secure raw blanks rigidly in a vise jaw, table-mounted clamps, or spindle chuck rotating jaws before starting automatic drilling cycles.
- Deselect Radius Compensation: Deselect cutter radius compensation (G41 or G42) with G40 prior to cycle execution to avoid Siemens Alarm 61815 or centerline positioning errors.
- Validate Dwell Integers: Program dwell times as whole integer milliseconds (e.g. P1500 for 1.5 seconds) on Fanuc and Mitsubishi systems to prevent decimal truncation and tool glazing.
- Confirm Modal Cancellation: Cancel modal cycles with G80 (or MCALL cancel on Siemens) to avoid unintended drilling plunges on subsequent positioning coordinates.
- Execute Single-Block Test: Verify safety clearances on the HMI coordinate screen by running a single-block dry run before initiating high-speed auto feeds.
Basic Concepts of Peck Drilling
The mechanical process of deep-hole peck drilling—periodically dividing deep axial cuts into smaller infeed steps and retracting to clear chip accumulation—is universally applied across Fanuc, Siemens, and Mitsubishi controllers to prevent tool wear, thermal fatigue, and drill breakage. Spot drilling is often executed first using a G81 spot drilling cycle to guide the deep-hole drill tip and prevent coordinate wandering.
By intermittently dividing deep axial cuts into multiple, smaller feed motions and retracting the tool completely out of the hole back to the safe Point R clearance level, G83 prevents the packing of chips within the drill flutes. This allows cutting fluid and coolant to wash away hot, abrasive chips and directly lubricate the tool tip. The G83 cycle is modally active, meaning it remains active until a G80 canned cycle cancel command is programmed.
This dramatic reduction in cutting friction and thermal fatigue extends the tool life of indexable and solid carbide drills, particularly when machining through tough, work-hardening alloys. During chip removal, the drill feeds to depth, executes a dwell if programmed, and then retracts completely out of the hole to the reference plane shifted by the safety clearance to evacuate chips. For materials that produce short chips, programmers can opt for the G73 high-speed peck drilling cycle which breaks chips by retracting by only a small, parameter-driven clearance distance without losing non-cutting travel time.
Command Structure and Syntax
The syntax of the deep-hole peck drilling cycle varies depending on the control system and mode selected. On Fanuc and Mitsubishi systems, G83 is a modal command that operates within Group 09. Once activated, the machine will execute the drilling cycle at the initial coordinate and repeat the sequence at any subsequent coordinate block until a cancel command is programmed. This syntax relies on specific letters to define coordinate offsets and machining behavior.
On Siemens Sinumerik controls, the programmer can choose between the native mode and the ISO Dialect mode. The native mode utilizes a parameter-driven technology cycle called CYCLE83, which must be preceded by a modal MCALL command. In ISO Dialect mode, the controller compiles a standard G83 G-code structure using Group 10 modal registers. Each of these structures requires careful configuration of axes, depths, clearances, and dwell times.
; Fanuc Standard Milling Format:
G98 (or G99) G83 X_ Y_ Z_ R_ Q_ D_ F_ K_ ;
; Fanuc Standard Turning Format (Face Drilling):
G83 X(U)_ C(H)_ Z(W)_ R_ P_ Q_ ,D_ F_ K_ M_ ;
; Siemens Native Mode:
MCALL CYCLE83 (RTP, RFP, SDIS, DP, DPR, FDEP, FDPR, DAM, DTB, DTS, FRF, VARI, _AXN, MDEP, _VRT, _DTD, _DIS1) ;
; Siemens ISO Dialect Mode:
G83 X(U)_ C(H)_ Z(W)_ R_ Q_ P_ F_ K_ M_ ;
; Mitsubishi Lathe Format:
G83 X/U_ C/H_ Z/W_ Rr Qq Pp Ff Kk Mm ;
; Mitsubishi Machining Center Special Format:
G83 Xx1 Yy1 Zz1 Rr1 Qq1 Ff1 Pp1, li1, Jj1 Dd1 Ee1 ;| Address / Parameter | Description | System / Units |
|---|---|---|
| X, Y (or U, V, C, H) | Coordinates of the hole center | Fanuc, Mitsubishi, Siemens ISO (mm or inches) |
| Z (or W) | Final depth coordinates (absolute or incremental) | Fanuc, Mitsubishi, Siemens ISO (mm or inches) |
| R (or Rr) | Point R clearance plane coordinate or incremental distance | Fanuc, Mitsubishi, Siemens ISO (mm or inches) |
| Q (or Qq) | Incremental depth of cut per peck (strictly positive) | Fanuc, Mitsubishi, Siemens ISO (mm or microns) |
| P (or Pp) | Dwell time at bottom of the hole | Fanuc, Mitsubishi, Siemens ISO (milliseconds, no decimal) |
| F (or Ff) | Cutting feedrate | Fanuc, Mitsubishi, Siemens ISO (mm/min or inch/min) |
| K (or Kk, LI, L) | Number of cycle repetitions | Fanuc, Mitsubishi, Siemens ISO (Integer 0 to 9999) |
| D (or ,D) | Relief / retract clearance amount | Fanuc, Mitsubishi (positive real) |
| RTP, RFP, SDIS | Retraction plane, reference plane, safety clearance | Siemens Native CYCLE83 (coordinates/real values) |
| DP, DPR, DTB | Absolute depth, relative depth, dwell time | Siemens Native CYCLE83 (coordinates/seconds/revolutions) |
| DAM, VARI, _AXN | Degression value, machining type, tool axis selection | Siemens Native CYCLE83 (parameters/integers) |
Brand Applications: Fanuc, Siemens, and Mitsubishi
Fanuc
On Fanuc turning and milling systems, the G83 cycle modal execution uses Group 09 registers. The cycle uses Parameter 5115 for standard retraction clearance.
A standard drilling block on a machining center is written as G90 G99 G83 X300.0 Y-250.0 Z-150.0 R-100.0 Q15.0 F120.0 K1 ; which drills absolute coordinates with a 15mm peck depth.
| Aspect | Details |
|---|---|
| Critical Parameters | Parameter No. 5101 Bit 2 (RTR) toggles standard chip removal (1) vs. high-speed chip breaking (0). Parameter No. 5115 defines default clearance distance d for standard peck. Parameter No. 5114 defines default clearance distance d for high-speed peck. Parameter No. 5185 specifies in-position check width during peck retraction. |
| Associated Alarms | Alarm PS0206 (AXIS SWITCHING IN RIGID MODE) occurs when active coordinate planes or drilling axes are changed without cancel. Alarm PS0200 (ILLEGAL S CODE COMMAND) triggers if spindle speed S exceeds active gear rotation limits. Alarm PS0368 (OFFSET REMAIN AT OFFSET COMMAND) triggers if parameter change occurs while offset is active. |
| Version Differences | Series 15 commands repetitions via address L, and Point R absolute coordinates are toggleable via RAB Parameter 5102 Bit 6. Series 16/30i uses address K for repetitions and defaults to incremental Point R coordinates. |
Siemens
On Sinumerik controls, the technological cycle CYCLE83 operates under G290 mode. In G291 ISO dialect mode, G83 operates as a Group 10 command using GUD7 variables.
A native command structure is written as MCALL CYCLE83 (155.0, 150.0, 1.0, 5.0, , 100.0, , 20.0, 1.0, 1.0, 1.0, 0, 3, 8.0, 0.8) ; which executes chip breaking.
| Aspect | Details |
|---|---|
| Critical Parameters | VARI determines chip breaking (0, retracting by _VRT) vs. chip removal (1, retracting to RFP + SDIS). DAM defines degression factor for decreasing peck depths. FRF scales the first peck feedrate. |
| Associated Alarms | Alarm 61101 (Reference plane defined incorrectly) triggers if RFP, RTP, and depth coordinates are inconsistent. Alarm 61815 (G40 not active) triggers if G41/G42 is active. Alarm 61800 (External CNC system missing) triggers if G291 is called when MD 18800 is disabled. Alarm 61102 (No spindle direction programmed) triggers if M03/M04 is missing. |
| Version Differences | Sinumerik 802D sl lacks support for inverse-time feedrate (G93) and features write-protected G-code reset variables like MD 20154. Sinumerik 840D sl supports full G-group screen displays and G93. |
Mitsubishi
On Mitsubishi CNCs, G83 is mapped as Face Deep Hole Drilling Cycle 1 for lathes or standard Peck Drilling for milling. The control reads Parameter 8013 for relief clearance.
An example is G83 X25.0 Z-14.5 R-3.0 Q5000 F200.0 M12 ; which drills to Z-14.5 with a 5mm peck depth and C-axis clamp M12 active.
| Aspect | Details |
|---|---|
| Critical Parameters | Parameter #8013 specifies retraction clearance amount. Parameter #19417 (Hole dec check 2) configures deceleration checks (0: no check, 1: check at cut point & bottom, 2: full check with sv024). Parameter #1184 (clmp_D) sets C-axis spindle unclamping dwell. |
| Associated Alarms | Program Error P411 (Axis name switching G111 active) triggers if G111 is executed while cycle is active. Program Error P652 (Sub Part System Control under high-accuracy mode) triggers if G122/G144 is issued while cycle is active. Program Error P33 (Simultaneous X and Z axis in G83.2) triggers if both axes are commanded in the same G83.2 block. |
| Version Differences | M800V/M80V series with software version A9 or later supports advanced cutting reduction (Jj2 subsequent reduction, Kk2 floor limit). Lathe systems map G83 to Z-axis drilling, while Milling systems map it to modal Group 09. |
Brand Comparison Analysis
| Topic | Fanuc | Siemens | Mitsubishi |
|---|---|---|---|
| Bimodal Program Format Switch Compiler | No bimodal switch compiler for canned cycles. | Bilingual parser via G290/G291 toggles between native CYCLE83 and G83 canned cycle modes. | Bilingual parser via G188/G189 dynamically reallocates G83 canned cycle tables. |
| Coordinate & Repetition Decoupling | Inline coordinate positioning and repeat counts (K or L). | Decouples coordinates from cycle using MCALL modal call and separate location subprograms or macros. | Inline coordinate positioning and repeat counts (K or LI). Special format permits inline axis check parameters. |
| Parameter-Level Retraction & Dwell Formats | Integer dwells (P in ms). Retraction type set globally via Parameter RTR. Clearance distance managed by Parameters 5114/5115. | Spindle-rev dwells (DTB < 0) or decimal seconds. Scales first feed rate (FRF) and degression (DAM) with decimals. | Integer dwells (Pp1 in ms, decimals truncated). Retraction clearance set by Parameter #8013. Unclamping dwell set by Parameter #1184. |
| Deceleration & Safety Checks | Managed globally via parameters. Retraction in-position check width controlled by Parameter 5185. | Retract _VRT and safety clearance SDIS. In-position checks governed by preprocessor variables. | Parameter #19417 (Hole dec check 2) configures deceleration checks (0: none, 1: cut point & bottom, 2: full check with sv024). |
Technical Analysis of Compiler and Coordinate Behaviors
A comparative analysis of canned cycle processing reveals three fundamental differences between Fanuc, Siemens, and Mitsubishi compiler architectures.
First, the compiler translation model for G83 cycle deactivation differs. Fanuc permits active canned cycles to be canceled on-the-fly using standard Group 01 motion commands. Specifying a Group 01 command like G00 or G01 in a subsequent block automatically cancels G83, behaving identically to an explicit G80. Conversely, Siemens native mode CYCLE83 is called via MCALL and remains active across subsequent blocks, completely ignoring G00 or G01 transitions until an explicit, standalone empty MCALL block is executed. Mitsubishi also requires G80 or G188 transitions to clear active cycle memory.
Second, the decoupling of coordinate positions from cycle blocks varies. Siemens native mode completely isolates the drilling technology cycle from the coordinates of hole centers. The MCALL CYCLE83 block defines only the drilling behavior, allowing coordinates or pattern macros (like HOLES2) to be listed on separate lines. Fanuc and Mitsubishi, however, write coordinates, repeat counts, and cycle parameters inline on the same block. Mitsubishi's Special Format even permits programmers to write axis in-position check widths directly inside the cycle block.
Third, parameter and dwell formats diverge. Fanuc and Mitsubishi utilize integer dwells specified in milliseconds (address P or Pp1), where decimals are either prohibited or truncated. Mitsubishi's Special Format truncates decimals, meaning P1.5 is compiled as 1ms. Siemens specifies bottom dwell (DTB) directly as real decimal seconds or spindle revolutions, and supports scaling parameters like feedrate factor (FRF) and degression (DAM) as real decimal percentages. Fanuc and Mitsubishi manage retraction clearances via parameters (Parameter 5115 for Fanuc, #8013 for Mitsubishi), whereas Siemens specifies safety clearance SDIS and retract _VRT directly in the program.
CNC Program Examples with Dry Run
Fanuc Canned Cycle Example
G90 G99 G83 X300.0 Y-250.0 Z-150.0 R-100.0 Q15.0 F120.0 K1 ;Dry Run
The machine executes a rapid traverse positioning (G00) in the XY plane to X300.0, Y-250.0. The Z-axis rapid traverses to the Point R clearance level of -100.0. The drill feeds at F120.0 to the first peck depth of Z-115.0 (calculated as R-100.0 minus Q15.0). The Z-axis rapid traverses back to the Point R level of -100.0 to clear chips and admit coolant. The Z-axis rapid traverses down to -114.5 (clearance distance d defined by Parameter 5115 as 0.5mm above the previous depth of -115.0). The Z-axis feeds at F120.0 for the next 15mm peck to depth Z-130.0. The Z-axis rapid traverses back to Point R (-100.0). The Z-axis rapid traverses down to -129.5 (clearance d). The Z-axis feeds at F120.0 to the final absolute depth of Z-150.0. The cycle completes, and the Z-axis rapid traverses back to Point R (-100.0) because G99 is active.
Siemens Technological Cycle Example
G290 ;
MCALL CYCLE83 (155.0, 150.0, 1.0, 5.0, , 100.0, , 20.0, 1.0, 1.0, 1.0, 0, 3, 8.0, 0.8) ;
X100.0 Y100.0 ;
MCALL ;Dry Run
The program enters native Siemens mode (G290). The modal call MCALL is activated for CYCLE83 with parameters: reference plane RFP=150.0, retraction plane RTP=155.0, safety clearance SDIS=1.0, final depth DP=5.0, first peck depth FDEP=100.0, degression DAM=20.0, dwell DTB=1.0s, feedrate factor FRF=1.0, machining type VARI=0 (chip breaking), tool axis _AXN=3 (Z-axis), retract _VRT=8.0mm, and path clearance _DIS1=0.8mm. On moving to coordinate X100.0 Y100.0, the Z-axis rapid traverses to the reference plane shifted by safety clearance (RFP+SDIS = 151.0). The Z-axis feeds at programmed feedrate to the first peck depth of 100.0. The Z-axis retracts by the chip-breaking distance _VRT (8.0mm) to break stringy chips, moving to Z-coordinate 108.0. The Z-axis rapid traverses down to 100.8 (which is 100.0 + _DIS1 0.8mm). The Z-axis feeds for the next peck. The peck depth is decremented by DAM=20.0, so the infeed is 80.0, reaching absolute coordinate 20.0. The Z-axis retracts by _VRT (8.0mm) to Z28.0. The Z-axis rapid traverses down to 20.8. The Z-axis feeds to the final depth coordinate of 5.0. The spindle dwells at the bottom for 1.0 second. The Z-axis rapid traverses back to the retraction plane RTP (155.0). The blank MCALL block cancels the modal cycle.
Mitsubishi Lathe Cycle Example
G83 X25.0 Z-14.5 R-3.0 Q5000 F200.0 M12 ;Dry Run
The machine tool performs rapid positioning (G00) in the XC plane to coordinate X25.0. The C-axis spindle clamping command M12 is executed, locking the spindle in position. The Z-axis rapid traverses to the Point R level (which is 3.0mm above the face: Z-3.0). The Z-axis feeds at F200.0 to the first peck depth of Z-8.0 (calculated as Point R minus Q5.0). The Z-axis rapid traverses back to the Point R level (Z-3.0) for standard chip removal. The Z-axis rapid traverses back down to Z-7.5 (safety clearance m defined by Parameter #8013 as 0.5mm). The Z-axis feeds at F200.0 to the final absolute depth of Z-14.5. The unclamp command M13 is automatically output by the control, and the spindle dwells for the duration configured in Parameter #1184 (clmp_D). The Z-axis rapid traverses back to the initial safety plane.
Error Analysis and Alarm Troubleshooting
| Brand | Alarm Code | Trigger Condition | Operator Symptom | Root Cause / Fix |
|---|---|---|---|---|
| Fanuc | Alarm PS0206 | Attempted axis or plane switching (e.g. from Z-axis to X-axis cycle) without canceling active canned cycle. | Axis travel halts, program execution stops, and the screen displays Alarm PS0206. | G83 modal cycle is still active in the system state. Execute a G80 canned cycle cancel block first before commanding the new axis or plane. |
| Fanuc | Alarm PS0200 | Programmed spindle speed (S) exceeds the maximum rotation limits of the gear configuration. | Program stops, spindle fails to rotate, and the screen displays Alarm PS0200. | Spindle speed limit exceeded. Verify speed limits in active gear range and reduce S value. |
| Fanuc | Alarm PS0368 | Attempted offset parameter change while offset values are active in registers. | Cycle execution halts, tool motion ceases, and the screen displays Alarm PS0368. | Active offsets must be cleared. Command tool offset cancellation first before attempting parameter changes. |
| Siemens | Alarm 61101 | Reference plane RFP, retraction plane RTP, and depth coordinates are inconsistent. | Control halts block pre-read, cycle fails to start, and the screen displays Alarm 61101. | Coordinates are logically incorrect (e.g. RTP is below depth). Correct plane coordinates in the CYCLE83 parameter list so RTP is above RFP and DP. |
| Siemens | Alarm 61815 | External G291 ISO Dialect mode cycle called while cutter radius compensation G41 or G42 is active. | Preprocessor halts execution, axis travel halts, and the screen displays Alarm 61815. | Cutter compensation is invalid in drilling modes. Deselect cutter radius compensation with G40 before calling G83. |
| Siemens | Alarm 61800 | G291 ISO dialect mode commanded but external language compilation is disabled on control. | Switching compiler fails, block compilation halts, and the screen displays Alarm 61800. | Option bit or compile register is disabled. Enable machine data parameter MD 18800 $MN_MM_EXTERN_LANGUAGE. |
| Siemens | Alarm 61102 | Spindle rotation M03 or M04 is missing from active registers during cycle call. | Program execution halts at cycle start, spindle remains stationary, and the screen displays Alarm 61102. | Spindle rotation must be initialized. Program spindle direction (M03/M04) and speed (S) before the cycle block. |
| Mitsubishi | Program Error P411 | Axis Name Switching command (G111) executed while G83 cycle is active. | Program halts, axis travel stops, and the screen displays Program Error P411. | Axis transformation cannot be commanded while modal cycles are active. Cancel cycle with G80 before commanding G111. |
| Mitsubishi | Program Error P33 | Both hole drilling axis X (or U) and Z (or W) commanded in the same G83.2 block. | Axis travel halts, program halts, and the screen displays Program Error P33. | Dual-axis drilling command is invalid for G83.2. Command axis target coordinates separately. |
| Mitsubishi | Program Error P923 | Coordinate rotation or 3D coordinate conversion (G68.1) called while G83 is active. | Compiler halts program, axis movements stop, and the screen displays Program Error P923. | Coordinate transformations cannot be initiated while canned cycle is active. Cancel the G83 cycle with G80 prior to calling G68.1. |
| Mitsubishi | Operation Error M01 0107 | Calculated cutting feedrate and spindle speed exceed maximum gear clamp rates. | Feed halts, spindle stops, and the screen displays Operation Error M01 0107. | Physical gear speed limits exceeded. Adjust speed or feedrate to within physical gear limits. |
Practical Application Note
Drill breakage and workpiece scrap occur if the operator resumes automatic program execution after a reset or emergency stop without canceling the active canned cycle registers. On Fanuc, Siemens, and Mitsubishi systems, G83 coordinates and drilling mode remain stored in the preprocessor registers after a reset. When automatic execution is restarted, the control interprets the next positioning coordinate as an active drilling block. This causes the tool-holding gantry or indexing turret to travel along a shifted trajectory, driving the drill directly into the vise jaw or table-mounted clamps. Setup operators must configure tailstock barrier safety envelopes on the NC interface screen and execute a manual G80 (or empty MCALL) to clear preprocessor registers before restarting.
Related Command Network
- G80: Cancels all active canned cycles, resetting the control to normal motion interpolation mode.
- G73: Executes high-speed peck drilling where the tool retracts by only a small clearance distance d for chip breaking rather than retracting fully to Point R.
- G81: Performs standard spot drilling or drilling without peck feeding.
- CYCLE830: Provides advanced deep-hole drilling on Siemens controls, including pilot-hole control, soft first cut, and through drilling with reduced feedrate.
- G83.2: Executes Deep Hole Drilling Cycle 2 on Mitsubishi lathe systems, permitting separate initial and subsequent peck increments.
Conclusion
Successful deep-hole drilling relies on precise clearance settings, correct modal cancellation, and verification of spindle status. Ensure all canned cycles are explicitly deactivated with G80 or MCALL before executing subsequent positioning coordinates to prevent unintended tool plunges into workpiece fixtures. Setting appropriate parameter-level check widths and dry-running programs in single-block mode ensures safe tool retraction and avoids costly collision crashes.
Frequently Asked Questions
How does the RTR parameter change G83 behavior on Fanuc controls?
The RTR parameter (Parameter 5101 Bit 2) toggles G83 between standard chip removal (RTR=1, where the drill retracts fully to Point R to evacuate chips) and high-speed chip breaking (RTR=0, where the drill retracts only by a small clearance distance d defined by Parameter 5114). To change the retract behavior without modifying G-code blocks, access the NC parameter page on the HMI and set Parameter 5101 Bit 2 to the desired binary state before running the program.
Why does a decimal point in address P or Pp1 cause tool breakage on Fanuc and Mitsubishi controls?
Fanuc and Mitsubishi compile dwell time (P or Pp1) as integer milliseconds, where decimals are either ignored or truncated. Specifying P1.5 on a Mitsubishi control parses the value as P1 (1 millisecond), making the dwell virtually nonexistent. This leads to immediate tool glazing and chip packing at the bottom of the hole. Always program dwells as integer milliseconds, writing P1500 for a 1.5-second dwell.
How does the Siemens degression factor (DAM) improve deep-hole drilling efficiency?
The DAM parameter in CYCLE83 allows subsequent peck depths to decrease dynamically as the hole gets deeper, preventing tool load buildup. Program DAM with a positive reduction increment (e.g. DAM=2.0 mm) or a negative decimal percentage (e.g. DAM=-0.8 to reduce each subsequent peck to 80% of the previous one). To apply this, insert a negative degression factor in your CYCLE83 block when drilling tough, work-hardening alloys to extend drill life.