Fanuc Canned Cycles Explained: G73, G81, G82, G83, G84 to G88, Address Words, Parameters 5121/5213 and Alarm 045

Canned cycles are the "one line, a whole sequence of moves" feature in FANUC programming – and where beginners get into the most trouble: forgetting G80, writing Q as 0, reversing G98/G99. Light cases scramble hole positions; bad cases crash the tool. This guide covers how to choose among the nine cycles, how to write the address words, the parameter ranges, and the three common alarms. For a one-page lookup see the canned-cycle cross-reference in further reading. The 5200–5209 definitions differ by machine – verify each against the manual for your control; Q is derived from material and drill diameter and confirmed by trial cutting, never a single universal number.

Sister article: FANUC canned cycles: nine cycles, address words and alarm 045 root causes. Related: Fanuc rigid tapping parameters 5200–5294, Fanuc Macro B guide, FANUC SERVO GUIDE and rigid tapping.

1.1 Get the three modal states right first

The three modal states to keep straight
ModalFunctionIf you forget it
G90 / G91Absolute / incremental, sets the datum for Z bottom and Q peckWrong datum -> the whole hole depth shifted
G98 / G99Return to initial plane / return to R planeWrong retract plane -> hit the fixture or scrape the part
G80Cancel canned cycleForgotten -> the next position drills again where it should not
广告

Table 1. The three modals define canned-cycle behaviour

Forgetting G80 is the number-one accident source: a canned cycle is modal, so once active, every following X/Y position executes a drill until G80 cancels. Cancel with G80 before tool changes and operations.

1.2 Address words: X/Y/Z/R/Q/P/F/K

AddressMeaningKey point
X / YHole positionOne cycle executes per position
ZHole bottomAffected by G90/G91
RRapid to R planeBoundary between rapid and cutting feed
QPeck depthRequired for G73/G83; must be on the same line as the G code
PDwell at bottomUnit set by parameter 5204 (ms or s)
FFeed rateCutting feed
KRepeat countFANUC uses K (some systems use L); with G91 for equally spaced arrays

Table 2. Canned-cycle address words (units and requirements follow the manual for your control)

K versus L: FANUC canned cycles use K for repeat count; some systems use L. Do not mix them. G91 + K makes an equally spaced hole array in one line, but confirm the R and Z datum first.

1.3 Nine cycles in one table

Choosing among the nine cycles
CyclePurposeBottom / retract behaviour
G81Standard drillFeed to bottom, rapid back to R plane
G82Drill with dwellDwell P at bottom (counterbore, spot face)
G83Deep-hole peckEach peck Q then fully retracts to R plane to clear chips
G73High-speed peckEach peck Q then retracts only slightly, no full chip break
G84Right-hand rigid tappingSpindle and Z synchronised, reversed on retract
G74Left-hand tappingReverse tapping
G85BoringFeed in, feed out (chip clearing)
G86BoringFeed in, spindle stop, rapid out
G87 / G88Deep-hole boring / manual retract boreNeeds spindle orientation / manual retract

Table 3. Choosing the nine cycles (exact motions follow the manual for your control)

1.4 G73 versus G83: retract distance decides chip clearing

The retract difference between G73 and G83
AspectG73 high-speed peckG83 deep-hole peck
After each peckRetracts only a little (breaks chip)Fully retracts to R plane
Chip clearingNo forced clearing, relies on chip breakingClears chips fully each peck
Use forShallow holes, short-chipping materialDeep holes (>5xD), long-chipping material (Al, Cu)

Table 4. How to choose between G73 and G83

In one line: deep holes and long chips mean G83. G73 chases speed but will pack chips and break the drill where clearing is poor.

1.5 How to set Q: give the rule, not a number

A common starting point for Q (peck depth) is Q ≈ 0.5–1 x D (drill diameter): smaller for steel, larger for aluminium. That is only a starting point – precision grades and drill materials can double it; derive it from material and tool diameter and confirm by trial cutting. Anyone who gives you a “universal Q value” without naming the material and diameter should not be copied.

1.6 G84 rigid tapping versus M29

In rigid tapping, the G84 cycle keeps spindle rotation and Z feed strictly synchronised (through the parameter chain – see rigid tapping parameters 5200–5294). Non-rigid tapping relies on the spindle encoder’s one-revolution signal for synchronisation compensation.

A power interruption or direction change mid-tap desynchronises Z from the thread – the classic rigid-tapping fault. After recovery you must re-establish synchronisation; never resume cutting directly.

1.7 Parameters: 5121 / 5213 / 5200–5209

Parameter ranges and alarms
广告
ParameterFunctionKey point
5121G73 cutting amountAffects each high-speed peck
5213G83 peck amountAffects the Q baseline for deep-hole pecking
5200–5209Z/R/retract and incremental modes per cycleDefinitions differ by machine – verify against the manual
5204P dwell unit (1 ms or 1 s)Wrong unit = dwell off by 1000 times

Table 5. Canned-cycle parameters (verify each against the manual for your control)

5204 is the silent killer: P = 500 means half a second if the unit is ms, or 500 seconds if it is s – downtime, crashes and scrap all follow from this. Confirm your machine’s 5204 setting before changing anything.

1.8 Alarm 045 / 073 / 074 root causes

AlarmMeaningRoot cause
045ADDRESS Q NOT FOUNDG73/G83 missing Q: Q typed as 0 or O, or written on the next line (Q must be on the same block as G73/G83)
073Program number already existsTrying to store an O number that is taken
074Program number out of rangeO number outside 1–9999

Table 6. Root causes of the three common alarms

045 is the most frequent: Q must be in the same block as G73/G83; Q0 (zero) or QO (letter O) are both rejected.

1.9 When the post-processor drops Q

A CAM shop changes its post and every hole now throws 045 – troubleshoot in this order: program -> post-processor -> parameters: first look at whether the G83 line in the generated NC code has a Q, then check the post configuration, and only then suspect parameters. Most cases are the post outputting Q on a separate line.

1.10 Safety and verification

For a new or modified cycle, dry-run / single-block to verify Z motion, R plane, hole bottom and retract before cutting metal. With G91 + K arrays, confirm the R and Z datum first or the whole array shifts. For rigid tapping, confirm synchronisation is healthy before cutting.

Frequently Asked Questions

What is the difference between G73 and G83, and which to use for deep holes?

G73 pecks with only a small retract and no full chip break, chasing speed; G83 retracts fully to the R plane each peck to clear chips. Deep holes (>5xD) and long-chipping material such as aluminium or copper need G83, or chips pack and the drill breaks.

Why do I get alarm 045 on a canned cycle, and how do I write Q?

045 is ADDRESS Q NOT FOUND – G73/G83 is missing Q. Common causes are typing Q as 0 or the letter O, or putting Q on the next line. Q must be in the same block as G73/G83.

What is the difference between G98 and G99, and what happens if I forget G80?

G98 returns to the initial plane, G99 to the R plane. Without G80 the cycle stays modal, so each following X/Y position drills again – wrong holes or a crash. Cancel with G80 before tool changes and new operations.

Last updated: 2026-11-19

Where to go next

Read the guide, get the right instrument, or walk the diagnosis through with someone — pick whichever you need.

© 版权声明
THE END
喜欢就支持一下吧
点赞10赞赏 分享
评论 抢沙发

请登录后发表评论

    暂无评论内容

CNC电气调试问题解答 | 数控机床电气工程师资料共享屋
CNC电气调试问题解答 | 数控机床电气工程师资料共享屋
CNC电气调试问题解答 | 数控机床电气工程师资料共享屋
CNC电气调试问题解答 | 数控机床电气工程师资料共享屋
CNC电气调试问题解答 | 数控机床电气工程师资料共享屋
CNC电气调试问题解答 | 数控机床电气工程师资料共享屋
图片-CNCShare | 数控电气技术中心
图片-CNCShare | 数控电气技术中心
图片-CNCShare | 数控电气技术中心
图片-CNCShare | 数控电气技术中心
图片-CNCShare | 数控电气技术中心
图片-CNCShare | 数控电气技术中心
Fanuc Canned Cycles Explained: G73, G81, G82, G83, G84 to G88, Address Words, Parameters 5121/5213 and Alarm 045-CNCShare | 数控电气技术中心
FANUC 固定循环怎么用?G81 / G82 / G83 / G73 / G84 / G85 / G86 / G87 / G88 九个循环一张表选对 + Q/R/P/K 地址字 + 参数 5121/5213 + 045 报警根因-CNCShare | 数控电气技术中心
SINUMERIK Servo Tuning: p1400, p1460, p1462, p1960 and p1656 — Reading the Bode Plot to Stop Servo Humming-CNCShare | 数控电气技术中心
SINUMERIK 828D / 840D sl 电机嗡鸣、振动怎么调?驱动侧 p1400 / p1460 / p1462 / p1960 自优化 / p1656 陷波 + Bode 图判读 + NC 侧 Kv 的先后顺序-CNCShare | 数控电气技术中心
SINUMERIK Drive Faults Explained: F30020, F30021, F30011, F07011 and A30010 — the 230xxx Mapping, r0949 Fault Values and First Checks-CNCShare | 数控电气技术中心
SINAMICS F 码怎么查?828D 上的 230020 到底是 F30020 —— F30001 / F30011 / F30021 / F07011 / A30010 逐条对照 + r0949 故障值读法 + 首选检查动作-CNCShare | 数控电气技术中心
Sinumerik F-Code Cross-Reference: F300xx / F0xxx / A3xxx Mapped to 230xxx Display Numbers-CNCShare | 数控电气技术中心
SINAMICS F 码 ↔ SINUMERIK 828D / 840D sl 显示号 四向对照总表:F 码 / 230xxx 六位号 / 故障原因 / 首选检查动作(每条可链)-CNCShare | 数控电气技术中心
FANUC PMC Scan Time: Why Inputs Get Missed and Timers Fire Early-CNCShare | 数控电气技术中心
FANUC PMC 扫描周期怎么导致信号漏采、定时器提前:中文现场排查-CNCShare | 数控电气技术中心
Schematic ↔ I/O Table ↔ PMC Ladder: Three-Way Cross-Reference Fault Tracing-CNCShare | 数控电气技术中心
电气原理图 ↔ I/O 分配表 ↔ PMC 梯形图三方对照:从报警反查到端子和元件的完整路径-CNCShare | 数控电气技术中心
文章精选
专心做好一件事
打造更优雅的WordPress主题-CNCShare | 数控电气技术中心
专心做好一件事
打造更优雅的WordPress主题