HEIDENHAIN TNC Fixed Cycle Parameter Reference: Cycle 200/203/230/251/252/4xx Q Parameters and FANUC G-Cycle Migration

When you program a HEIDENHAIN TNC control, the most frequent action is looking up what a cycle's Q parameter actually means. The official TNCguide is a PDF: not searchable inside your browser, not deep-linkable. The "HEIDENHAIN G-code cycle lists" circulating on Chinese websites are copied from one another with cycle numbers only and no Q-parameter meanings. This page organizes the drilling, pocket-milling, probing, tool-measurement and turning cycle families into a searchable reference with row-level anchors, and adds a function-level migration map to FANUC G-cycles.

One high-frequency error corrected first: many online tables label Q212 as “finishing allowance” and Q213 as “corner allowance”. Per the official TNCguide, Q212 is the DECREMENT (infeed reduction per plunge) and Q213 is the number of chip breaks before retracting (NR OF BREAKS BEFORE RETRACTING); the real side/floor finishing allowances are Q368 / Q369. Copying the wrong table deforms deep-hole drilling cycle behavior. Every parameter name must be checked against the manual for iTNC530 / TNC620 / TNC640 / TNC7 individually — the same cycle can use different parameter names across generations; your machine manual wins.

广告

Sister article: HEIDENHAIN TNC Fixed Cycle Parameter Reference (Chinese); related: Heidenhain touch-probe calibration: iTNC 530 uses MP, TNC 640/TNC7 uses Cfg, HEIDENHAIN iTNC 530 vs TNC 620/640/TNC7 differences and migration, Fanuc Canned Cycles Explained: G73, G81-G88, Fanuc Canned Cycle Parameter Table.

27.1 Search by family first, not by number: the cycle map

HEIDENHAIN cycle family map

HEIDENHAIN fixed cycles are grouped into families, not scattered numbers. Identify the family before looking up a parameter so the Q-parameter meanings line up.

Table 1 HEIDENHAIN fixed-cycle family map (number ranges vary slightly by generation; check your manual)

FamilyCycle rangeWhat it doesWhere parameters land
Drilling / tapping200-209, 240, 241, 262-267drill, ream, center drill, tap, bore-millQ200/Q201/Q202/Q203/Q204/Q206/Q210/Q211
Pocket milling230-233, 251-258, 262-265, 271-277slots, rectangular/round pockets, islandsQ215/Q218/Q219/Q368/Q369/Q370/Q351
Contour20, 24, 25, 27-29, 39, 276contour millingQ2/Q6/Q7/Q9 (GLOBAL DEF 110/111)
Part probing400-419 (datum), 420-431 (measurement)datum setting, hole/plane measurementQ260/Q261/Q320/Q321-Q324/Q303
Tool measurement480-485 (new) / 31-33 (old)tool length / radius by touch-off deviceTOOL.T columns CUT/DIRECT/R-OFFS/L-OFFS
Turning800-892OD, facing, thread, grooveturning-cycle specific Q parameters

How to read: the iTNC 530 uses the 4xx probing cycles, while newer TNC640 / TNC7 use the 14xx series — the two systems cannot share cycle numbers. Tool measurement 480-483 corresponds functionally to old numbers 31-33, but status parameters live in different places; see Heidenhain touch-probe calibration and TNC generation differences.

27.2 Common Q parameters first: learn these before any specific cycle

Common Q parameters

Drilling and pocket cycles share a core set of Q parameters. Learn this “common vocabulary” once and the per-cycle entries need no repetition.

Table 2 Common Q parameters for drilling (per official TNCguide; incremental/absolute nature per your manual)

ParameterOfficial nameNatureMeaning
Q200SET-UP CLEARANCEincrementalTool tip to workpiece surface; enter positive
Q201DEPTHincrementalSurface to hole bottom; normally negative; sign sets working direction, =0 skips cycle
Q202PLUNGING DEPTHincrementalInfeed per cut; need not divide depth evenly
Q203SURFACE COORDINATEabsoluteWorkpiece surface coordinate in spindle axis
Q2042ND SET-UP CLEARANCEincrementalRetract height clear of workpiece/fixtures
Q206FEED RATE FOR PLUNGING–mm/min, or FAUTO / FU / FZ
Q210DWELL TIME AT THE TOP–Seconds at setup clearance after chip-removal retract
Q211DWELL TIME AT DEPTH–Seconds at hole bottom

Correction box (the four most-miscopied online)

  • Q212 = DECREMENT (value subtracted from Q202 after each infeed), not “finishing allowance”; works with Q205 minimum plunging depth.
  • Q213 = NR OF BREAKS BEFORE RETRACTING, not “corner allowance”; works with Q256 retract distance and Q257 chip-breaking depth.
  • Real side/floor allowances are Q368 (side) / Q369 (floor) in pocket cycles, not Q212/Q213.
  • Q204 is officially incremental (clearance above the Q203 surface); some third-party tables call it an “absolute second safety height” — check your manual; the two appear as different numbers in the program.

The displayDepthErr trap: the manual is explicit — the machine parameter displayDepthErr decides whether the TNC raises an error on a positive depth. With a positive depth entered, the TNC reverses the pre-positioning calculation and rapid-traverses the tool to the setup clearance BELOW the workpiece surface. Do not flip the depth sign by feel; write depth negative (down) by default.

27.3 Drilling family entry by entry: 200 / 201 / 202 / 203 / 204 / 206 / 207 / 208 / 209

Drilling is the most-looked-up family. Similar function does not mean identical Q parameters: 201 reaming retracts at feed, 203 universal drilling uses chip breaking, 206/207 are tapping — do not cross-apply parameters.

Table 3 Drilling/tapping cycle roles (Q meanings in 27.2; ranges per your manual)

CycleOfficial nameKey differenceMain Q parameters
CYCL DEF 200DRILLINGStandard drill, multi-plunge to depthQ200/Q201/Q202/Q203/Q204/Q206/Q210/Q211
CYCL DEF 201REAMING (G201)Reamer in/out at feed, spindle does not stopQ200/Q201/Q206/Q211
CYCL DEF 202CENTER DRILLINGShallow center holeQ200/Q201/Q203/Q204/Q206
CYCL DEF 203UNIVERSAL DRILLING (G203)Chip breaking / retract, first choice for deep holes200 set plus Q212/Q213/Q205/Q208/Q256/Q395
CYCL DEF 204Deep-hole class (generation-dependent)Definitions differ across manuals — check your machinePer your manual
CYCL DEF 206TAPPINGTapping with retractQ200/Q201/Q203/Q204/Q206 plus pitch parameters
CYCL DEF 207RIGID TAPPINGSpindle/feed synchronizedSync parameters per your manual
CYCL DEF 208BORE MILLING (G208)Helical interpolation for large boresQ335 nominal dia / Q342 roughing dia / Q351 direction / Q334 feed per revolution
CYCL DEF 209Thread-milling class (generation-dependent)Check your manualPer your manual

Q335 vs Q342 (the pair most confused in Cycle 208): Q335 is the nominal bore diameter; if nominal equals tool diameter, the TNC bores straight to depth with no helical interpolation. Q342 is the roughing diameter; any value above 0 stops the TNC from checking the bore/tool diameter ratio, allowing rough-milling of holes larger than twice the tool diameter. Q351 = +1 climb milling, -1 up-cut (0 is also treated as climb).

27.4 Pocket milling family: 230 / 231 / 251 / 252 / 256 / 257 and Q2xx reuse

Pocket cycles have many Q parameters but high reuse: the Q200/Q201/Q203/Q204 positioning set repeats across the family; what distinguishes cycles is shape + allowance + path parameters.

Table 4 Pocket/slot cycles and dedicated Q parameters

CycleOfficial nameShape / dedicated parametersNotes
CYCL DEF 230SLOT MILLINGslot length/width/directionMill a long slot in one pass
CYCL DEF 231Slot milling (multi-pass / generation-dependent)Per your manualHigh-speed deep-hole/slot class, function near FANUC G73
CYCL DEF 251RECTANGULAR POCKETQ218 1st side / Q219 2nd side / Q220 corner radius / Q224 rotationQ215 sets operation (rough/finish)
CYCL DEF 252CIRCULAR POCKET (G252)Q223 circle diameterQ215 sets operation
CYCL DEF 256Rect/round pocket (generation-dependent)Per your manualIncluded in TNC640 pocket-cycle global data range
CYCL DEF 257Pocket class (generation-dependent)Per your manualSame; do not copy across machines

Family reuse rules: Q368 (side allowance) and Q369 (floor allowance) take effect only when a finishing operation is defined; Q370 is the path overlap factor (Q370 x tool radius = stepover k, range 0.1-1.9999); Q351 climb +1 / up-cut -1; Q366 plunging strategy (0 vertical, 1 helical, 2 reciprocating). These are the GLOBAL DEF 105/110/111 common data and can be reused family-wide.

27.5 Probing 400-431 and tool measurement 480-484: change parameters in the right place

Probing splits into 400-419 datum setting (build coordinate system), 420-431 measurement (measure size); tool measurement is 480-484 (new) / 31-33 (old). The three groups store parameters in different places — the classic mistake is “editing a measurement parameter inside a datum cycle.”

Table 5 Probing and tool-measurement families (iTNC530 4xx system; TNC640/TNC7 partly 14xx)

RangePurposeTypical cyclesKey Q parameters
400-419Part datum, set zero410 datum inside rectangle, 411 datum outsideQ321/Q322 center, Q323/Q324 sides, Q260 clearance, Q261 measuring height, Q305 table number
420-431Part measurement420 angle, 421 hole, 422 outside circle, 423/424 rectangle, 430 bolt circle, 431 planeQ260 clearance, Q261 measuring height, Q303 value transfer
480-484Tool measurement480 calibrate TT, 481 length, 482 radius, 483 both, 484 calibrate IR TTStatus in TOOL.T columns (CUT/DIRECT/R-OFFS/L-OFFS), Q199 status (new numbers)

Where parameters actually live: on iTNC530, global probe behavior (feed, pre-positioning, max traverse, safety clearance) is in machine parameters MP6120 / MP6130 / MP6140 / MP6150 / MP6151 etc.; on TNC640 / TNC7 this moved to the Cfg configuration tables — exactly the “iTNC530 uses MP, TNC640/TNC7 uses Cfg, don’t edit the wrong place” point stressed in Heidenhain touch-probe calibration. If you change safety clearance in a datum cycle and nothing happens, you most likely edited the wrong generation’s location.

广告

27.6 Turning family 800-892: a separate system, do not mix with milling

The 800-892 turning family covers TNC turning cycles (OD, facing, thread, groove, center drilling, etc.) with a different Q-parameter system from milling, normally seen on turn-mill machines with C/Y axes. Check first that the machine is in turning mode and the cycle is in the 8xx range, then verify each against the machine’s turning manual. This page does not expand the turning Q table to avoid cross-machine copy errors.

27.7 FANUC G-cycle migration map: one line per pair, parameters are not directly convertible

FANUC cycle migration map

Moving from FANUC to HEIDENHAIN, the common question is “I used G83, which Cycle replaces it?” The table gives function-level approximate mapping — note this is an analogy: FANUC G + address words and HEIDENHAIN CYCL DEF + Q parameters are different systems; parameters cannot be converted one by one.

Table 6 FANUC G-cycle to HEIDENHAIN Cycle approximate functional map (not directly convertible)

FANUCFunctionHEIDENHAIN approximateWhat does not convert
G81Standard drillingCycle 200G98/G99 return mode vs Q204 second clearance
G82Counterbore (dwell at bottom)Cycle 201 / 200 + Q211201 is reaming semantics; dwell is Q211
G83Deep-hole peck drillingCycle 203R point vs Q203/Q200; different chip-break system
G73High-speed deep-hole drillingCycle 231 classDifferent retract-distance definition
G84TappingCycle 206 / 207Rigid-tapping sync parameters per your manual
G85Boring (feed in/out)Cycle 230 / 231 classBore-milling 208 is helical, different semantics
G86Boring (rapid retract)Cycle 22x classNumber range varies widely across generations
G87 / G88Back boring / manual boringCycle 241 classLatter is thread-milling class, only functionally close

Migration discipline: first align on “what motion this cycle must produce”, then fill every Q parameter against your manual; never take a FANUC R point, Z value or K value and divide by a factor to get a HEIDENHAIN value. The FANUC side is covered in Fanuc Canned Cycles Explained and Fanuc Canned Cycle Parameter Table.

27.8 Common pitfalls: sign, feed semantics, diameter split, climb/up-cut

Cycle common pitfalls

Table 7 Four frequent mis-fills and the correct practice

PitfallSymptomCorrect practice
Depth sign reversalPositive depth reverses pre-positioning; tool rapids below surfaceWrite depth negative (down); displayDepthErr only raises an error, it does not fix it
FAUTO / FU semanticsTreating FAUTO as a fixed feed valueFAUTO/FU/FZ mean “compute feed from the tool table”; algorithm per your manual
Q335 / Q342 splitBore larger than twice tool diameter raises an errorFill Q342 roughing diameter to release the ratio check
Q351 climb/up-cutUp-cut entered as -1, or 0 assumed to be up-cut+1 climb, -1 up-cut, 0 is treated as climb

27.9 Table declaration and usage discipline

Declaration: parameter meanings in this table are checked against the individual manuals for iTNC530 / TNC620 / TNC640 / TNC7; the same cycle can use different parameter names across generations. All ranges and examples are subject to your machine manual and shop-floor test cutting. Cycle numbers and Q definitions follow the manual shipped with your machine — this page is a lookup entry point, not a replacement for the manual.

Usage discipline: (1) locate the family, then look up the number; (2) obtain official manuals only through HEIDENHAIN’s official channels and your machine documents — this site does not host manual PDFs; (3) when cross-checking CAM-posted cycles, the post output and your machine manual win; (4) dry-run the first article single-block for deep holes, bore-milling and probing, confirming clearance and depth sign before batch running.

Frequently Asked Questions

What is the difference between HEIDENHAIN Cycle 200 and Cycle 201?

Cycle 200 is standard drilling with multi-plunge to depth, using Q202 for infeed per cut and Q210/Q211 for dwell. Cycle 201 is reaming (G201): the reamer travels in and out at feed with the spindle not stopping, and has no multi-plunge chip-breaking logic. You cannot apply 200 parameters to reaming; feed and retract semantics differ.

When do Q200 and Q204 differ?

Q200 is the setup clearance from tool tip to workpiece surface, the approach height before the cycle starts. Q204 is the second setup clearance, the retract height clear of workpiece/fixtures, officially incremental (above the surface). With tall fixtures or clamps, Q204 must be clearly above Q200; for simple flat drilling they can differ without being equal. Check both against your manual.

Can HEIDENHAIN drilling cycles be used like FANUC G81, and how do parameters convert?

Not directly. G81 is G-code plus R-point/Z-value address words; Cycle 200 is CYCL DEF plus Q parameters. Functionally G81 maps to Cycle 200, but the FANUC R point splits into HEIDENHAIN Q203 (surface coordinate) + Q200 (clearance), Z depth becomes Q201 (mind the negative sign), and return mode is expressed through Q204. Refill every parameter against your manual and dry-run the first article single-block.

Last updated: 2026-11-20

Where to go next

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

Also available in Chinese: 海德汉 TNC 固定循环参数速查表:Cycle 200/203/230/251/252/256/257/4xx/48x 逐个 Q 参数含义 + 与 FANUC G 循环迁移
The original Chinese version — same procedure, with the full field notes.
© 版权声明
THE END
喜欢就支持一下吧
点赞9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
SINUMERIK 828D / 840D sl vs FANUC vs Mitsubishi M80 Parameter Cross-Reference (Aligned by Function)-CNCShare | 数控电气技术中心
828D / 840D sl ↔ FANUC ↔ 三菱 M80 常用参数三方对照总表(按功能对齐,不按号段对齐)-CNCShare | 数控电气技术中心
HEIDENHAIN TNC Fixed Cycle Parameter Reference: Cycle 200/203/230/251/252/4xx Q Parameters and FANUC G-Cycle Migration-CNCShare | 数控电气技术中心
海德汉 TNC 固定循环参数速查表:Cycle 200/203/230/251/252/256/257/4xx/48x 逐个 Q 参数含义 + 与 FANUC G 循环迁移-CNCShare | 数控电气技术中心
机床为什么要预热?热变形与首件精度漂移:三处热源 + 20 分钟预热协议 + 主轴油温与环境温度设定 + 热伸长诊断方法-CNCShare | 数控电气技术中心
Replacing a FANUC Servo Motor: Parameters 2020, 2022 and 2021, Re-measuring Inertia and Re-verifying Compensation-CNCShare | 数控电气技术中心
FANUC 换伺服电机后参数怎么回写?2020 / 2022 / 2021 + 惯量比重测 + 编码器方向与对位 + 三步验收-CNCShare | 数控电气技术中心
SINUMERIK Servo Alarms 25000, 25010 and 25201: Which Layer to Troubleshoot First-CNCShare | 数控电气技术中心
828D / 840D sl 伺服报警 25000 / 25010 / 25201 怎么分层?先看 NC 报警还是 F 码-CNCShare | 数控电气技术中心
Mitsubishi MT Works2 / MR Configurator2: Official Download Path, Modules and Servo Parameters-CNCShare | 数控电气技术中心
三菱 MT Works2 / MR Configurator2 哪里下载?伺服调参上位机三大模块、怎么连 MR-J4/J5、能改哪些参数与三大下载坑-CNCShare | 数控电气技术中心
SINUMERIK 828D Tool Management NC-PLC Interface Explained: DB4300, Three Tables and the Drum-Magazine Wrong-Tool Case-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