SINUMERIK 828D G290 vs G291: DIN and ISO Mode Side by Side

If one NC program runs and another does not on the same 828D, check the programming language before blaming the drive. Siemens' own ISO programming manual states that G290 activates the Siemens NC programming language (commonly called DIN mode in workshops) and G291 activates the ISO dialect. Switching does not change the active tool, tool offsets or work offsets, but G290 and G291 must each be programmed alone in an NC block, and the two languages must not be mixed in the same block.

Chinese version: 828D G290 / G291 guide; related: 828D cycle alarms 61000 / 62000 / 65xxx, Setting Data vs Machine Data on 828D, 828D PLC Programming Tool and basic blocks, CNC alarm number formats by brand.

11.1 What G290 and G291 actually switch

G290 and G291 mode switching
CommandActive languageOfficial wordingWorkshop shorthand
G290Siemens NC programming languageSiemens NC programming language activeBack to DIN mode
G291ISO dialectISO Dialect NC Programming language activeEnter ISO mode

Table 1: official names and shop-floor terms

广告

The Siemens manual adds three boundaries: in ISO dialect mode only ISO G functions may be programmed, not Siemens G functions; ISO dialect and Siemens language cannot be mixed in one NC block; and switching between ISO dialect M and ISO dialect T with a G command is not possible. The often-repeated statement that the two modes “recognize each other” has a narrower meaning: a subprogram written in Siemens mode can be called from ISO mode, and shell cycles implicitly switch to Siemens mode. It is not permission to mix statements freely.

11.2 Why machine builders switch modes

Three sources commonly meet on one machine: legacy programs written in Siemens/DIN style, customer programs migrated from FANUC or other controls using G71/G70 and T0101, and machine-builder cycles that are Siemens standard cycles. Mode switching solves the syntax source problem only. It does not validate the tool, the work offset or the process.

Because the official manual says the active tool, tool compensation and work offsets are not influenced by the switch, those values remain in force. Verify them before switching, not after a collision.

11.3 Side-by-side: program header, tool, spindle, contour, cycle

DIN and ISO side by side

This is a structural comparison, not an automatic translation table. Cycle availability, address meaning and default G groups depend on the installed control version and machine-builder configuration.

ItemSiemens / DIN styleISO dialect styleKey point
HeaderG290 plus G54 / WORKPIECE setupG291 plus G90 G40 G99 as configuredMode switch alone in its own block
Tool changeT1 D1 or builder-defined blockT0101 if MD10888/10889/10890 configuredT0101 is not universal by default
SpindleS800 M3S800 M03ISO mode follows the ISO G-code table
PositioningG0 X… Z…G00 X… Z…Same intent, different language environment
ContourG1 / G2 / G3 plus Siemens cyclesG01 / G02 / G03 plus G71/G70Never mix both G-code sets in one block
Finishing cycleCYCLE952 and related cyclesG70 P… Q…Cycle calls implicitly switch mode
EndM30M30Resulting mode follows parameters and call context

Table 2: shape of equivalent actions, for structure only

11.4 The G71 / G70 trap exists in both styles

G71 roughing and G70 finishing

A Siemens CNC4YOU example shows an 828D program that prepares a simulated workpiece with G290, enters ISO mode with G291, then uses G71 U… R…, G71 P… Q… U… W… F… and G70 P… Q… F… for rough and finish turning. Two conclusions follow:

  1. G71/G70 can be used in ISO mode, but that does not make the whole program language-neutral.
  2. Siemens cycles can be called from ISO structure because the shell cycle switches mode internally; Siemens statements cannot be dropped into the same ISO block.

Sign of U for outside versus inside contours, P-Q contour monotonicity and allowance direction sit at the boundary between ISO rules and cycle implementation. Verify them with a graphical simulation and dry run before cutting metal.

11.5 Three real mixed-programming failures

Three mixed-mode failure points
FailureSymptomAction
Both languages in one blockAlarm or unexpected interpretationPut G290 / G291 in separate blocks and keep each block single-language
T0101 not configuredTool change or offset does not activate as expectedCheck MD10888 / 10889 / 10890 bit 2 / 20310 bit 16 and the tool table H column
Parameter changed but no resetValue changed, behaviour did notPerform the required NCK reset; obtain machine-builder approval first
广告

Table 3: the three most common 828D mixed-mode errors

The CNC4YOU example also mentions U/W incremental programming with MD10881, removing ( ), O program numbers and % from imported ISO programs, and using channel user variable _ZSFI for G92 thread run-out. These belong to that example, not to every 828D default.

11.6 CYCLE62 and CYCLE952 in an ISO-structured program

Siemens’ example uses CYCLE62 and CYCLE952 inside a program whose visible structure is largely ISO style. The control still executes standard Siemens cycles: a shell cycle is called through the main program, the Siemens mode is selected automatically, and G codes changed inside the shell cycle are restored at the end through the SAVE attribute. DISPLOF keeps the displayed block language frozen on ISO while the cycle runs internally in Siemens mode.

Before relying on this, check three things: the cycle is in the standard scope for that channel, the call point is correctly placed relative to the mode switch, and the machine builder has not overridden the cycle.

11.7 A safe dual-style workflow

  1. Back up the original program and relevant machine data; record current mode, G54, tool and offsets.
  2. Use a standalone G290 block for Siemens-side preparation and a standalone G291 block to enter ISO.
  3. Keep every NC block in one language; treat Siemens cycle calls through their shell-cycle rules.
  4. Run graphical simulation, then dry run; focus on tool changes, approach/retract, U/W direction and the P-Q contour range.
  5. Run the first article in single-block mode with the feed hold ready.
  6. Return the machine to its agreed default mode before handing the control to the next operator.

11.8 Scope and compliance

  • Mode definitions, the standalone-block rule, the ban on same-block mixing, unchanged tool/offsets and implicit shell-cycle switching come from the Siemens SINUMERIK 840D sl / 828D ISO Turning Programming Manual and the ISO dialects function manual.
  • G71/G70, CYCLE62, CYCLE952 and machine-data hints come from a Siemens CNC4YOU worked example. They are example settings, not a substitute for the delivered manual or machine-builder approval.
  • No manual text is reproduced and no cracked software, drive link or pirated archive is offered. Back up before edits and validate the first article under a qualified operator.

Frequently Asked Questions

What is the difference between G290 and G291 on an 828D?

G290 activates the Siemens NC programming language, often called DIN mode; G291 activates the ISO dialect. Use G291 for customer ISO programs or G71/G70 style code, and G290 for Siemens-native statements and standard cycles. Each command must stand alone in its own NC block.

Can G71 roughing be used in G291 mode?

Yes, but G71/G70 belong to the ISO dialect, so the surrounding program must follow ISO rules. Siemens standard cycles called from ISO structure switch mode through a shell cycle. The difference is syntax and modality, not the ability to cut. Simulate U/W direction, P-Q range and allowances before the first part.

Why do some programs run on the same 828D while others fail?

Check mode consistency, standalone G290/G291 blocks, whether ISO-style T0101 is configured through machine data, and whether an NCK reset followed parameter changes. These four checks explain most “same machine, different result” cases.

Last updated: 2026-11-16

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: SINUMERIK 828D G290 G291 怎么切?DIN 写法与 ISO 写法逐行对照
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5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 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
数控电气调试软件与官方手册哪里下载?FANUC / 西门子 / 三菱 / 海德汉 官方入口与版本对应-CNCShare | 数控电气技术中心
SINUMERIK 828D G290 vs G291: DIN and ISO Mode Side by Side-CNCShare | 数控电气技术中心
SINUMERIK 828D G290 G291 怎么切?DIN 写法与 ISO 写法逐行对照-CNCShare | 数控电气技术中心
SINUMERIK 840D sl to S7-1500: NCVAR Selector, PROFINET Names and Alarm 150202-CNCShare | 数控电气技术中心
SINUMERIK 840D sl 与 S7-1500 怎么通讯?PROFINET 设备名 + NCVAR Selector 从 PLC 读写 MD 全流程-CNCShare | 数控电气技术中心
CNC Alarm Message Chinese Reference: 120 Common English Phrases and a 30-Second Triage Method-CNCShare | 数控电气技术中心
Five Peripheral Alarm Clusters on CNC Machines: Coolant, Lubrication, Chip Conveyor, Air and Hydraulics - From English Alarm Text to PMC Feedback to Action-CNCShare | 数控电气技术中心
数控机床英文报警中文对照(120 条句式样例)+ 看到英文报警后 30 秒定位该查哪个点-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