Siemens SINUMERIK 808D User manual

© Siemens AG 2017. All rights reserved
01/2017 1
SINUMERIK 808D
SINUMERIK 808D, SINUMERIK 808D ADVANCED
Programming and Operating Manual (ISO Turning/Milling)
User Manual
Legal information
Warning notice system
This manual contains notices you have to observe in order to ensure your personal safety, as well as to prevent damage to property. The
notices referring to your personal safety are highlighted in the manual by a safety alert symbol, notices referring only to property damage
have no safety alert symbol. These notices shown below are graded according to the degree of danger.
DANGER
indicates that death or severe personal injury will result if proper precautions are not taken.
WARNING
indicates that death or severe personal injury may result if proper precautions are not taken.
CAUTION
indicates that minor personal injury can result if proper precautions are not taken.
NOTICE
indicates that property damage can result if proper precautions are not taken.
If more than one degree of danger is present, the warning notice representing the highest degree of danger will be used. A notice warning of
injury to persons with a safety alert symbol may also include a warning relating to property damage.
Qualified Personnel
The product/system described in this documentation may be operated only by
personnel qualified
for the specific task in accordance with
the relevant documentation, in particular its warning notices and safety instructions. Qualified personnel are those who, based on their
training and experience, are capable of identifying risks and avoiding potential hazards when working with these products/systems.
Proper use of Siemens products
Note the following:
WARNING
Siemens products may only be used for the applications described in the catalog and in the relevant technical documentation. If products
and components from other manufacturers are used, these must be recommended or approved by Siemens. Proper transport, storage,
installation, assembly, commissioning, operation and maintenance are required to ensure that the products operate safely and without any
problems. The permissible ambient conditions must be complied with. The information in the relevant documentation must be observed.

Programming and Operating Manual (ISO Turning/Milling)
201/2017
Preface
Applicable products
This manual is valid for the following control systems:
Control system
Software version
SINUMERIK 808D ADVANCED T (Turning)
SINUMERIK 808D ADVANCED M (Milling)
V4.7.4: PPU161.3/PPU160.2 with spindle/feed servo system
SINUMERIK 808D (Turning)
SINUMERIK 808D (Milling)
V4.7.4: PPU141.2 with feed servo system
Documentation components and target audience
End-user documentation
Target audience
Programming and Operating Manual (Turning)
Programmers and operators of turning machines
Programming and Operating Manual (Milling)
Programmers and operators of milling machines
Programming and Operating Manual (ISO Turning/Milling)
Programmers and operators of turning/milling machines
Programming and Operating Manual (Manual Machine Plus
(MM+), Turning)
Programmers and operators of turning machines
Diagnostics Manual
Mechanical and electrical designers, commissioning engi-
neers, machine operators, and service and maintenance
personnel
Manufacturer/service documentation
Target audience
Commissioning Manual
Installation personnel, commissioning engineers, and ser-
vice and maintenance personnel
Function Manual
Mechanical and electrical designers, technical professionals
Parameter Manual
Mechanical and electrical designers, technical professionals
Service Manual Mechanical and electrical designers, technical profession-
als, commissioning engineers, and service and maintenance
personnel
Readme file
Third-party software - Licensing terms and copyright information
My Documentation Manager (MDM)
Under the following link you will find information to individually compile your documentation based on the Siemens content:
www.siemens.com/mdm
Standard scope
This manual only describes the functionality of the standard version. Extensions or changes made by the machine tool
manufacturer are documented by the machine tool manufacturer.
Technical support
Country
Hotline
1)
Further service contact information:
•Worldwide Web site:
https://support.industry.siemens.com/cs/ww/en/
•Chinese Web site:
http://www.siemens.com.cn/808D
Germany
[phone]
China [phone]
1) You can find more hotline information at the worldwide Web site given above.
EC Declaration of Conformity
The EC Declaration of Conformity for the EMC Directive can be found on the Internet at
http://www.siemens.com/automation/service&support.
Here, enter the number "
67385845
" as the search term or contact your local Siemens office.

Programming and Operating Manual (ISO Turning/Milling)
01/2017 3
Table of contents
Preface...................................................................................................................................................................2
1 Fundamental safety instructions ..............................................................................................................................5
1.1 General safety instructions......................................................................................................................5
1.2 Industrial security ....................................................................................................................................6
2 Fundamentals of programming................................................................................................................................6
2.1 Introductory remarks................................................................................................................................6
2.1.1 Siemens mode ........................................................................................................................................6
2.1.2 ISO dialect mode.....................................................................................................................................7
2.1.3 Switching between Siemens and ISO modes..........................................................................................7
2.1.4 Display of the G code ..............................................................................................................................8
2.1.5 Maximum number of axes/axis identifiers................................................................................................8
2.1.6 Selecting G code system A, B or C .........................................................................................................8
2.1.7 Programming the decimal point...............................................................................................................8
2.1.8 Comments.............................................................................................................................................10
2.1.9 Block skip ..............................................................................................................................................11
2.1.10 Notes on the PLC interface signal address representation....................................................................11
2.2 Prerequisites for the feed ......................................................................................................................11
2.2.1 Rapid traverse .......................................................................................................................................11
2.2.2 Path feed (F function)............................................................................................................................11
2.2.3 Linear feed (G98/G94)...........................................................................................................................14
2.2.4 Inverse-time feed (G93) (milling only)....................................................................................................14
2.2.5 Revolutional feedrate (G99/G95)...........................................................................................................14
3 Turning.................................................................................................................................................................14
3.1 G code table..........................................................................................................................................14
3.1.1 SINUMERIK ISO dialect turning mode A...............................................................................................14
3.1.2 SINUMERIK ISO dialect turning mode B...............................................................................................16
3.1.3 SINUMERIK ISO dialect turning mode C...............................................................................................18
3.2 Travel commands..................................................................................................................................20
3.2.1 Interpolation commands ........................................................................................................................20
3.2.1.1 Rapid traverse (G00).............................................................................................................................20
3.2.1.2 Linear interpolation (G01)......................................................................................................................22
3.2.1.3 Circular interpolation (G02, G03)...........................................................................................................23
3.2.1.4 Contour definition programming and insertion of chamfers and radii ....................................................26
3.2.1.5 Cylindrical interpolation (G07.1) ............................................................................................................27
3.2.1.6 Polar coordinates interpolation (G12.1, G13.1) (TRANSMIT)................................................................28
3.2.2 Reference point approach with G functions...........................................................................................30
3.2.2.1 Reference point approach with intermediate point (G28) ......................................................................30
3.2.2.2 Checking the reference position (G27)..................................................................................................31
3.2.2.3 Reference point approach with reference point selection (G30)............................................................31
3.2.3 Use of the thread cutting function..........................................................................................................32
3.2.3.1 Thread cutting with constant lead (G32)................................................................................................32
3.2.3.2 Interlinking of threads (G32)..................................................................................................................34
3.2.3.3 Cutting of multiple-start threads (G32)...................................................................................................34
3.2.3.4 Thread cutting with variable lead (G34).................................................................................................36
3.3 Measuring commands ...........................................................................................................................37
3.3.1 The coordinate system ..........................................................................................................................37
3.3.1.1 Machine coordinate system (G53).........................................................................................................37
3.3.1.2 Workpiece coordinate system (G50) .....................................................................................................38
3.3.1.3 Resetting the tool coordinate system (G50.3) .......................................................................................38
3.3.1.4 Selection of a workpiece coordinate system (G54 to G59)....................................................................38
3.3.1.5 Writing work offset/tool offsets (G10).....................................................................................................39
3.3.2 Defining the input modes for the coordinate values...............................................................................40
3.3.2.1 Diameter and radius programming for the X-axis ..................................................................................40
3.3.2.2 Input inch/metric (G20, G21) .................................................................................................................40
3.3.3 Time-controlled commands (G04) .........................................................................................................41
3.3.4 Tool offset functions ..............................................................................................................................41
3.3.4.1 Tool offset data memory........................................................................................................................41
3.3.4.2 Tool length compensation .....................................................................................................................42

Programming and Operating Manual (ISO Turning/Milling)
401/2017
3.3.4.3 Tool nose radius compensation (G40, G41/G42).................................................................................. 42
3.3.5 S-, T-, M- and B functions ..................................................................................................................... 46
3.3.5.1 Spindle function (S function) ................................................................................................................. 46
3.3.5.2 Constant cutting rate (G96, G97) .......................................................................................................... 47
3.3.5.3 Tool change with T functions (T function) ............................................................................................. 48
3.3.5.4 Additional function (M function)............................................................................................................. 48
3.3.5.5 M functions of spindle control (M19, M29) ............................................................................................ 49
3.3.5.6 M functions for subroutine calls (M98, M99) ......................................................................................... 49
3.3.5.7 Macro call via M function....................................................................................................................... 49
3.3.5.8 M functions (M08, M09) ........................................................................................................................ 50
3.4 Additional functions............................................................................................................................... 50
3.4.1 Program-support functions.................................................................................................................... 50
3.4.1.1 Fixed cycles (G90, G92, G94)............................................................................................................... 50
3.4.1.2 Multiple repetitive cycles (G70 to G76) ................................................................................................. 58
3.4.1.3 Drilling cycle (G80 to G89).................................................................................................................... 71
3.4.2 Programmable data input...................................................................................................................... 78
3.4.2.1 Changing the tool offset value (G10)..................................................................................................... 78
3.4.2.2 M function for calling subroutines (M98, M99) ...................................................................................... 79
3.4.3 Eight-digit program number (M98, G65/G66)........................................................................................ 80
3.4.4 Measuring functions (G31).................................................................................................................... 81
3.4.5 Macro programs.................................................................................................................................... 81
3.4.5.1 Differences with subroutines................................................................................................................. 82
3.4.5.2 Macro program call (G65, G66, G67).................................................................................................... 82
3.4.6 Special functions................................................................................................................................... 87
3.4.6.1 G05 ....................................................................................................................................................... 87
3.4.6.2 Switchover modes for DryRun and skip levels...................................................................................... 87
4 Milling...................................................................................................................................................................88
4.1 G code table.......................................................................................................................................... 88
4.2 Drive commands ................................................................................................................................... 90
4.2.1 Interpolation commands........................................................................................................................ 90
4.2.1.1 Cylindrical interpolation (G07.1)............................................................................................................ 90
4.2.1.2 Rapid traverse (G00)............................................................................................................................. 92
4.2.1.3 Linear interpolation (G01) ..................................................................................................................... 93
4.2.1.4 Circular interpolation (G02, G03) .......................................................................................................... 94
4.2.1.5 Contour definition programming and addition of chamfers or radiuses ................................................. 96
4.2.1.6 Helical interpolation (G02, G03)............................................................................................................ 97
4.2.2 Reference point approach with G functions .......................................................................................... 98
4.2.2.1 Reference point approach with intermediate point (G28)...................................................................... 98
4.2.2.2 Checking the reference position (G27).................................................................................................. 99
4.2.2.3 Reference point approach with reference point selection (G30) ........................................................... 99
4.3 Motion commands............................................................................................................................... 100
4.3.1 The coordinate system........................................................................................................................ 100
4.3.1.1 Machine coordinate systems (G53)..................................................................................................... 100
4.3.1.2 Workpiece coordinate system (G92)................................................................................................... 101
4.3.1.3 Resetting the tool coordinate system (G92.1)..................................................................................... 101
4.3.1.4 Selection of a workpiece coordinate system (G54 to G59) ................................................................. 101
4.3.1.5 Writing work offset/tool offsets (G10) .................................................................................................. 102
4.3.1.6 Local coordinate system (G52) ........................................................................................................... 103
4.3.1.7 Selection of the plane (G17, G18, G19).............................................................................................. 103
4.3.1.8 Parallel axes (G17, G18, G19)............................................................................................................ 104
4.3.1.9 Rotation of the coordinate system (G68, G69).................................................................................... 104
4.3.1.10 3D rotation (G68/G69)......................................................................................................................... 105
4.3.2 Defining the input modes of the coordinate values ............................................................................. 106
4.3.2.1 Absolute/incremental dimensioning (G90, G91).................................................................................. 106
4.3.2.2 Inch/metric input (G20, G21)............................................................................................................... 107
4.3.2.3 Scaling (G50, G51) ............................................................................................................................. 107
4.3.2.4 Programmable mirroring (G50.1, G51.1)............................................................................................. 109
4.3.3 Time-controlled commands (G04)....................................................................................................... 111
4.3.4 Tool offset functions............................................................................................................................ 111
4.3.4.1 Tool offset data memory ..................................................................................................................... 111
4.3.4.2 Tool length compensation (G43, G44, G49) ....................................................................................... 112
4.3.4.3 Cutter radius compensation (G40, G41, G42)..................................................................................... 113
4.3.4.4 Collision detection............................................................................................................................... 116
4.3.5 S-, T-, M- and B functions ................................................................................................................... 119

Programming and Operating Manual (ISO Turning/Milling)
01/2017 5
4.3.5.1 Spindle function (S function)................................................................................................................119
4.3.5.2 Tool function........................................................................................................................................119
4.3.5.3 Additional function (M function) ...........................................................................................................119
4.3.5.4 M functions of spindle control (M19, M29)...........................................................................................120
4.3.5.5 M functions for subroutine calls (M98, M99)........................................................................................120
4.3.5.6 Macro call via M function.....................................................................................................................121
4.3.5.7 M functions (M08, M09).......................................................................................................................121
4.3.6 Controlling the feedrate .......................................................................................................................122
4.3.6.1 Compressor in ISO dialect mode.........................................................................................................122
4.3.6.2 Exact stop (G09, G61), continuous-path mode (G64), and tapping (G63)...........................................122
4.4 Additional functions .............................................................................................................................123
4.4.1 Program supporting functions..............................................................................................................123
4.4.1.1 Fixed drilling cycles (G73, G74, G76, G80 to G87, G89).....................................................................123
4.4.1.2 High-speed deep hole drilling cycle with chip breakage (G73)............................................................126
4.4.1.3 Fine drilling cycle (G76).......................................................................................................................128
4.4.1.4 Drilling cycle, counterboring (G81) ......................................................................................................130
4.4.1.5 Countersink drilling cycle (G82)...........................................................................................................132
4.4.1.6 Deep hole drilling cycle with chip removal (G83).................................................................................133
4.4.1.7 Boring cycle (G85)...............................................................................................................................134
4.4.1.8 Boring cycle (G86)...............................................................................................................................136
4.4.1.9 Boring cycle - reverse countersinking (G87)........................................................................................137
4.4.1.10 Boring cycle (G89)...............................................................................................................................139
4.4.1.11 "Drilling a right-hand thread without any compensating chuck" cycle (G84)........................................140
4.4.1.12 "Drilling a left-hand thread without any compensating chuck" cycle (G74)..........................................142
4.4.1.13 Left or right tapping cycle (G84/G74)...................................................................................................144
4.4.1.14 Deselection of a fixed cycle (G80).......................................................................................................146
4.4.1.15 Program example with a tool length compensation and fixed cycles...................................................146
4.4.2 Programmable data input (G10)..........................................................................................................148
4.4.2.1 Changing the tool offset value.............................................................................................................148
4.4.2.2 M function for calling subroutines (M98, M99).....................................................................................148
4.4.3 Eight-digit program number (M98, G65/G66) ......................................................................................149
4.4.4 Polar coordinates (G15, G16)..............................................................................................................149
4.4.5 Measuring functions ............................................................................................................................150
4.4.5.1 Measuring with "delete distance-to-go" (G31) .....................................................................................150
4.4.5.2 "Tool life control" function....................................................................................................................152
4.4.6 Macro programs ..................................................................................................................................152
4.4.6.1 Differences with subroutines ...............................................................................................................152
4.4.6.2 Macro program call (G65, G66, G67) ..................................................................................................152
4.4.6.3 Macro call via G function (G21)...........................................................................................................157
4.4.7 Special functions .................................................................................................................................159
4.4.7.1 Contour repetition (G72.1, G72.2) .......................................................................................................159
4.4.7.2 Switchover modes for DryRun and skip levels ....................................................................................161
1
Fundamental safety instructions
1.1
General safety instructions
WARNING
Danger to life if the safety instructions and residual risks are not observed
If the safety instructions and residual risks in the associated hardwar
e documentation are not observed, accidents involving
severe injuries or death can occur.
•Observe the safety instructions given in the hardware documentation.
•
Consider the residual risks for the risk evaluation.
WARNING
Danger to life or malfunctions of the machine as a result of incorrect or changed parameterization
As a result of incorrect or changed parameterization, machines can malfunction, which in turn can lead to injuries or death.
•Protect the parameterization (parameter assignments) against unauthorized access.
•
Respond to possible malfunctions by applying suitable measures (e.g. EMERGENCY STOP or EMERGENCY OFF).

Programming and Operating Manual (ISO Turning/Milling)
601/2017
1.2
Industrial security
Note
Industrial security
Siemens provides products and solutions with industrial security functions that support the secure operation of plant
s,
systems, machines and networks.
In order to protect plants, systems, machines and networks against cyber threats, it is necessary to implement
– and
continuously maintain
– a holistic, state-of-the-art industrial security concept. Siemens products and s
olutions only represent
one component of such a concept.
The customer is responsible for preventing unauthorized access to its plants, systems, machines and networks. Systems,
machines and components should only be connected to the enterprise network or the internet if and to the extent necessary
and with appropriate security measures (e.g. use of firewalls and network segmentation) in place.
Additionally, Siemens’ guidance on appropriate security measures should be taken into account. For more information
about
industrial security, please visit:
Industrial security (
http://www.siemens.com/industrialsecurity).
Siemens’ products and solutions undergo continuous development to make them more secure.
Siemens strongly
recommends to apply product updates as soon as available and to always use the latest product versions. Use of product
versions that are no longer supported, and failure to apply latest updates may increase customer’s exposure to cyber
th
reats.
To stay informed about product updates, subscribe to the Siemens Industrial Security RSS Feed at:
Industrial security (
http://www.siemens.com/industrialsecurity).
WARNING
Danger to life as a result of unsafe operating states resulting from software manipulation
Software manipulations (e.g. viruses, trojans, malware or worms) can cause unsafe operating states in your system that
may lead to death, serious injury, and property damage.
•Keep the software up to date.
•Incorporate the automation and drive components into a holistic, state-of-the-art industrial security concept for the
installation or machine.
•Make sure that you include all installed products into the holistic industrial security concept.
•Protect files stored on exchangeable storage media from malicious software by with suitable protection measures, e.g.
virus scanners.
2
Fundamentals of programming
WARNING
Danger to life and/or damage to machine due to insecure part programs
Running an insecure part program on your machine may cause unexpected attacks to the machine, which in turn can lead
to death, personal injuries, and/or machine damage.
•Make sure you use part programs that come from trusted sources.
2.1
Introductory remarks
2.1.1
Siemens mode
The following conditions are valid in Siemens mode:
●The default of the G commands can be defined for each channel via the machine data 20150
$MC_GCODE_RESET_VALUES.
●No language commands from the ISO dialects can be programmed in Siemens mode.

Programming and Operating Manual (ISO Turning/Milling)
01/2017 7
2.1.2
ISO dialect mode
The following conditions are valid in the active ISO dialect mode:
●ISO dialect mode can be set with machine data as the default setting of the control system. The control system reboots
by default in ISO dialect mode subsequently.
●Only G functions from the ISO dialect can be programmed; programming of Siemens G functions is impossible in ISO
Mode.
●The ISO dialect and Siemens language cannot be mixed in the same NC block.
●G commands cannot be used to switch between ISO dialect M and ISO dialect T.
●Subroutines that are programmed in Siemens mode can be called.
●If Siemens functions are to be used, switch the control system to Siemens mode first.
Note
Switching from Siemens mode to ISO dialect mode does not change the default value 0x04
of MD10890
EXTERN_TOOLPROG_MODE.
•
0x04
: select the tool offset only with an H number in ISO dialect mode.
•0: select the tool offset only with a D number in ISO dialect mode.
2.1.3
Switching between Siemens and ISO modes
The control system supports the following two programming language modes:
●Siemens language mode
●ISO dialect mode
Note that the active tool, tool offsets and workpiece offsets are not influenced by the mode changeover.
Switchover through G functions
The following G functions can be used to switch between Siemens mode and ISO dialect mode:
●G290 - Siemens NC programming language active
●G291 - ISO Dialect NC Programming language active
G290 and G291 must be programmed alone in an NC block.
Switchover on the HMI
Operating sequence
+
1.
Select the desired operating area.
2.
Press this softkey on the PPU. The control system automatically starts the mode change
from Siemens mode to ISO dialect mode. After the changeover, "ISO" is shown on the u
p-
per left corner of the screen.
To change from ISO mode back to Siemens mode, press the same softkey again.

Programming and Operating Manual (ISO Turning/Milling)
801/2017
2.1.4
Display of the G code
The G code is displayed in the same language type (Siemens or ISO dialect) as the relevant current block display. If the
display of the blocks is suppressed with DISPLOF, the G codes continue to be displayed in the language type of the active
block.
Example
The G functions of ISO dialect mode are used to call the Siemens standard cycles. To do this, DISPLOF is programmed at
the start of the relevant cycle; this way the G functions that are programmed in ISO dialect language continue to be
displayed.
PROC CYCLE328 SAVE DISPLOF
N10 ...
...
N99 RET
Procedure
The Siemens shell cycles are called via main programs. Siemens mode is selected automatically by calling the shell cycle.
With DISPLOF, the block display is frozen on calling the cycle; the display of the G code continues in ISO mode.
The G codes that were changed in the shell cycle are reset to their original status at the end of the cycle with the "SAVE"
attribute.
2.1.5
Maximum number of axes/axis identifiers
The maximum number of axes in ISO dialect mode is 9. The axis identifiers for the first three axes are defined with X, Y and
Z permanently. All other axes can be identified with letters A, B, C, U, V and W.
2.1.6
Selecting G code system A, B or C
ISO dialect T differentiates between G code systems A, B, and C. By default, the G code system A is active. Via the
MD10881 $MN_MM_EXTERN_GCODE_SYSTEM, the G code system A, B or C is selected as follows:
$MN_MM_EXTERN_GCODE_SYSTEM = 0: G code system B
$MN_MM_EXTERN_GCODE_SYSTEM = 1: G code system A
$MN_MM_EXTERN_GCODE_SYSTEM = 2: G code system C
G code system A
If the G code system A is active, then G91 is unavailable. In this case, an incremental axis movement with the address
characters U, V and W is programmed for axes X, Y and Z. The address characters U, V and W are not available in this
case as axis identifiers, and as a result, the maximum number of axes reduces to 6.
The address H is used for programming the incremental movements of the C-axis in the G code system A.
In order for the shell cycle to work in the correct G code system, the corresponding system must be entered in GUD variable
_ZSFI[39].
Note
•
If not otherwise noted, the manual in hand describes G code system A.
•For the differences between G code systems A, B, and C, see Section "G code table (Page 14)".
2.1.7
Programming the decimal point
In ISO Dialect mode, there are two notations for evaluating the programmed values without decimal point:
●
Pocket calculator notation
Values without decimal point are interpreted as mm, inch or degree.
●
Standard notation
Values without decimal points are multiplied with the conversion factor.

Programming and Operating Manual (ISO Turning/Milling)
01/2017 9
Complete the setting via MD10884 EXTERN_FLOATINGPOINT_PROG.
Note
Switching from Siemens mode to ISO
dialect mode does not change the current setting of MD10884
EXTERN_FLOATINGPOINT_PROG.
There are two different conversion factors,
IS-B
and
IS-C.
This evaluation refers to the addresses X, Y, Z, U, V, W, A, B, C, I,
J, K, Q, R, and F.
Complete the setting over MD10886 EXTERN_INCREMENT_SYSTEM.
Example:
Linear axis in mm:
●X 100.5
Corresponds to value with decimal point: 100.5 mm
●X 1000
–Pocket calculator notation: 1000 mm
–Standard notation:
IS-B: 1000 * 0.001= 1 mm
IS-C: 1000 * 0.0001 = 0.1 mm
ISO dialect turning
See the following table for different conversion factors for IS-B and IS-C.
Address
Unit
IS-B
IS-C
Linear axis
mm
inch
0.001
0.0001
0.0001
0.00001
Rotary axis
Degree
0.001
0.0001
F feed G94 (mm/inch per min.) mm
inch
1
0.01
1
0.01
F feed G95 (mm/inch per rotation)
$MC_EXTERN_FUNCTION_MASK
Bit8 = 0
Bit8 = 1
mm
inch
mm
inch
0.01
0.0001
0.0001
0.000001
0.01
0.0001
0.0001
0.000001
F thread lead mm
inch
0.0001
0.000001
0.0001
0.000001
C chamfer mm
inch
0.001
0.001
0.0001
0.0001
R radius. G10 toolcorr mm
inch
0.001
0.001
0.0001
0.0001
I. J, K interpolation parameters mm
inch
0.001
0.001
0.0001
0.0001
G04 X or U
0.001
0.001
A contour angle
0.001
0.001
G76, G92 thread cutting cycle
$MC_EXTERN_FUNCTION_MASK
Bit8 = 0 F as feed such as G94, G95
Bit8 = 1 F as thread lead

Programming and Operating Manual (ISO Turning/Milling)
10 01/2017
Address
Unit
IS-B
IS-C
G84, G88 tapping cycle
$MC_EXTERN_FUNCTION_MASK
Bit9 = 0 G95 F
Bit8 = 1 G95 F
mm
inch
mm
inch
0.01
0.0001
0.0001
0.000001
0.01
0.0001
0.0001
0.000001
ISO dialect milling
See the following table for different conversion factors for IS-B and IS-C.
Address
Unit
IS-B
IS-C
Linear axis mm
inch
0.001
0.0001
0.0001
0.00001
Rotary axis
Degree
0.001
0.0001
F feed G94 (mm/inch per min.) mm
inch
1
0.01
1
0.01
F feed G95 (mm/inch per rev.) mm
inch
0.01
0.0001
0.01
0.0001
F thread lead mm
inch
0.01
0.0001
0.01
0.0001
C chamfer mm
inch
0.001
0.0001
0.0001
0.00001
R radius, G10 toolcorr mm
inch
0.001
0.0001
0.0001
0.00001
Q mm
inch
0.001
0.0001
0.0001
0.00001
I, J, K interpolation parameters mm
inch
0.001
0.0001
0.0001
0.00001
G04 X or U
s
0.001
0.001
A contour angle
Degree
0.001
0.0001
G74, G84 tapping cycles
$MC_EXTERN_FUNCTION_MASK
Bit8 = 0 F as feed such as G94, G95
Bit8 = 1 F as thread lead
2.1.8
Comments
In ISO dialect mode, brackets are interpreted as comment signs. In Siemens mode, ";" is interpreted as comment. To
simplify matters, an ";" is also understood as comment in ISO dialect mode.
If the comment start sign "(" is used inside a comment again, the comment is ended only if all the open brackets are closed
again.
Example:
N5 (comment) X100 Y100
N10 (comment(comment)) X100 Y100
N15 (comment(comment) X100) Y100
X100 Y100 is executed in blocks N5 and N10, but only Y100 in block N15, because the first bracket is closed only after
X100. Everything up to that point is interpreted as a comment.

Programming and Operating Manual (ISO Turning/Milling)
01/2017 11
2.1.9
Block skip
The sign of skipping or suppression of blocks "/" can be used at any convenient position in a block, that is, even in the
middle of the block. If the programmed block skip level is active on the date of the compilation, the block is not compiled
from this point up to the end of the block. An active block skip level has the same effect as a block end.
Example:
N5 G00 X100. /3 YY100 --> Alarm 12080 "Syntax error"
N5 G00 X100. /3 YY100 --> no alarm, if block skip level 3 is active
Block skip signs within a comment are not interpreted as block skip signs
Example:
N5 G00 X100. (/3 Part1) Y100
;the Y axis is traversed even when the block skip level 3 is active
The block skip levels /1 to /9 can be active. Block skip values <1 and >9 lead to alarm 14060 "Impermissible skip level for
differential block skip".
The function is mapped to the existing Siemens skip levels. Unlike the ISO Dialect original, "/" and "/1" are separate skip
levels that must also be activated separately.
Note
The "0" in "/0" can be omitted.
2.1.10
Notes on the PLC interface signal address representation
Currently, PLC interface signal addresses are represented by the V structure on the HMI while the manual shows them by
the DB structure.
See the following table for the relationship between the two representations.
V Structure
DB Structure
Access
Example
Example
Access
Bit
V38000002.1
DB3800.DBX2.1
Bit
Byte VB38000002 DB3800.DBB2 Byte
Word
VW38000002
DB3800.DBW2
Word
Double Word
VD38000004
DB3800.DBD4
Double word
2.2
Prerequisites for the feed
The following Section describes the feed function with which the feedrate (covered path per minute or per rotation) of a
cutting tool is defined.
2.2.1
Rapid traverse
Rapid traverse is used for positioning (G00) as well as for manual traverse with rapid traverse (JOG). In rapid traverse, each
axis is traversed with the rapid traverse rate set for the individual axes. The rapid traversing rate is defined by the machine
manufacturer and it is specified by the machine data for the individual axes. As the axes traverse independently of each
other, each axis reaches its target point at a different time. Hence, the resulting tool path is generally not a straight line.
2.2.2
Path feed (F function)
Note
Unless otherwise specified, the unit "mm/min" is always used for the feedrate of the cutting tool in this documentation.
The feed, with which a tool should be traversed in case of linear interpolation (G01) or circular interpolation (G02, G03), is
programmed with the address character "F".
After the next address character "F", the feed of the cutting tool is specified in "mm/min".
The permissible range of the F value is given in the documentation of the machine manufacturer.

Programming and Operating Manual (ISO Turning/Milling)
12 01/2017
Possibly, the feed is restricted upward by the servo-system and by the mechanics. The maximum feed is set through the
machine data and is restricted before exceeding the value defined there.
The path feed is generally composed of the individual speed components of all geometry axes participating in the movement
and refers to the center point (see following images).
Turning:
Linear interpolation with two axes:
Circular interpolation with two axes:

Programming and Operating Manual (ISO Turning/Milling)
01/2017 13
Milling
Linear interpolation with two axes:
Circular interpolation with two axes:
In 3D interpolation, the feed of the resulting straight lines programmed with F are maintained in the space.

Programming and Operating Manual (ISO Turning/Milling)
14 01/2017
Note
If "F0" is programmed and the function "Fixed feedrates" is not activated in the block, then the alarm 14800 "C
hannel %1
Set %2 programmed path velocity is less than or equal to zero" is given off.
2.2.3
Linear feed (G98/G94)
On specifying G98 for turning/G94 for milling, the feed given after the address character F is executed in the mm/min,
inch/min or degree/min unit.
2.2.4
Inverse-time feed (G93) (milling only)
On specifying G93, the feed given after the address character F is executed in the 1/min unit. G93 is a modally effective G
function.
Example
N10 G93 G1 X100 F2 ;
i.e., the programmed path is traversed within half a minute.
2.2.5
Revolutional feedrate (G99/G95)
On entering G99 for turning/G95 for milling, the feed is executed in the mm/revolution unit or inch/revolution related to the
master spindle.
Note
All of the commands are modal. If the G feed command is switched between G98 and G99 for turning or among G93, G94,
and G95 for milling, th
e path feed must be reprogrammed. The feed can also be specified in degree/revolution for the
machining with rotary axes.
3
Turning
3.1
G code table
3.1.1
SINUMERIK ISO dialect turning mode A
Name
Index
Description
Format
01. G-Group (modal)
G0
1
Rapid traverse
G00 X... Z... ;
G1
2
Linear motion
G01 X... Z... F... ;
G2
3
Circle/helix in clockwise direction
G02(G03) X(U)... Z(W)... I... K... (R...)
F... ;
G3
4
Circle/helix in counterclockwise direction
G32
5
Thread cutting with constant lead
G32 X (U)... Z (W)... F... ;
G90
6
Longitudinal turning cycle
G.. X... Z... F...
G92
7
Thread cutting cycle
G... X... Z... F... ;
G94 8 Radial cutting cycle G... X... Z... F... ;
G34
9
Thread cutting with variable lead
G34 X (U)... Z (W)... F... K... ;
02. G-Group (modal)
G96
1
Constant cutting rate on
G96 S...
G97
2
Constant cutting rate off
G97 S...
04. G-Group (modal)
G68
1
Dual slide/turret on

Programming and Operating Manual (ISO Turning/Milling)
01/2017 15
Name
Index
Description
Format
G69
2
Dual slide/turret off
05. G-Group (modal)
G98
1
Linear feed
G99
2
Revolutional feedrate
06. G-Group (modal)
G20
1
Input system inch
G21
2
Input system metric
07. G-Group (modal)
G40
1
Deselection of cutter radius compensation
G41
2
Compensation left of contour
G42
3
Offset to right of contour
08. G-Group (modal)
10. G-Group (modal)
G80
1
Drilling cycle off
G80;
G83 2 Front face deep hole drilling G83 X(U)... C(H)... Z(W)... R... Q... P...
F... M... ;
G84 3 Front face tapping G84 X(U)... C(H)... Z(W)... R... P... F...
M... K... ;
G85 4 Front face drilling cycle G85 X(U)... C(H)... Z(W)... R... P... F...
K... M... ;
G87 5 Side surface deep hole drilling G87 Z(W)... C(H)... X(U)... R... Q... P...
F... M... ;
G88 6 Side surface tapping G88 Z(W)... C(H)... X(U)... R... P... F...
M... K... ;
G89 7 Side drilling G89 Z(W)... C(H)... X(U)... R... P... F...
K... M... ;
12. G-Group (modal)
G66
1
Macro module call
G66 P... L... <Parameters>;
G67
2
Delete macro-modal call
G67 P... L... <Parameters>;
14. G-Group (modal)
G54
1
Selecting work offset
G55
2
Selecting work offset
G56
3
Selecting work offset
G57
4
Selecting work offset
G58 5 Selecting work offset
G59
6
Selecting work offset
16. G-Group (modal)
G17
1
XY plane
G18
2
ZX plane
G19
3
YZ plane
18. G-Group (non-modal)
G4
1
Dwell time in [s] or spindle revolutions
G04 X...; or G04 P...;
G10
2
Write work offset/tool offset
G10 L2 Pp X... Z... ;
G28
3
1. Reference point approach
G28 X... Z... ;
G30
4
2./3./4. Reference point approach
G30 Pn X... Z... ;
G31
5
Delete measuring with distance-to-go
G31 X... Y... Z... F_;
G52
6
Programmable work offset

Programming and Operating Manual (ISO Turning/Milling)
16 01/2017
Name
Index
Description
Format
G65
7
Macro call
G65 P_ L_ ;
G70
8
Finishing cycle
G70 P... Q... ;
G71
9
Stock removal cycle, longitudinal axis
G71 U... R... ;
G72
10
Stock removal cycle, transverse axis
G72 W... R... ;
G73
11
Closed cutting cycle
G73 U... W... R... ;
G74
12
Multiple repetitive grooving cycles in the longitudinal axis
G74 R... ;
G75 13 Multiple repetitive grooving cycles in the transverse axis G75 R... ; or G75 X(U)... Z(W)... P...
Q... R... F... ;
G76
14
Multiple thread cutting cycle
G76 P... (m, r, a) Q... R... ;
G50
15
Set actual value
G92 (G50) X... Z... ;
G27
16
Referencing check (under development)
G27 X... Z... ;
G53
17
Approach position in machine coordinate system
G53 X... Z... ;
G07.1 18 Cylindrical interpolation G07.1 A (B, C) r;
G07.1 A (B, C) 0 ;
G5
20
High-speed cycle cutting
G05 Pxxxxx Lxxx ;
G30.1
21
Reference point position
-
G5.1
22
High-speed cycle -> Call of CYCLE305
-
G50.3
23
Delete actual value, reset the WCS
G60
24
directed positioning
21. G-Group (modal)
G13.1
1)
1
TRANSMIT OFF
G12.1
2
TRANSMIT ON
31. G-Group (modal)
G290
1
Select Siemens mode
-
G291
2
Select ISO dialect mode
-
3.1.2
SINUMERIK ISO dialect turning mode B
Name
Index
Description
Format
01. G-Group (modal)
G0
1
Rapid traverse
G00 X... Y... Z... ;
G1
2
Linear motion
G01 X... Z... F... ;
G2
3
Circle/helix in clockwise direction
G02(G03) X(U)... Z(W)... I... K... (R...)
F... ;
G3
4
Circle/helix in counterclockwise direction
G33
5
Thread cutting with constant lead
G33 X (U)... Z (W)... F... ;
G77
6
Longitudinal turning cycle
G.. X... Z... F...
G78
7
Thread cutting cycle
G... X... Z... F... ;
G79
8
Face turning cycle
G... X... Z... F... ;
G34
9
Thread cutting with variable lead
G34 X (U)... Z (W)... F... K... ;
02. G-Group (modal)
G96
1
Constant cutting rate on
G96 S...
G97
2
Constant cutting rate off
G97 S...
03. G-Group (modal)
G90
1
Absolute programming
G91
2
Incremental programming
04. G-Group (modal)
G68
1
Dual slide/turret on

Programming and Operating Manual (ISO Turning/Milling)
01/2017 17
Name
Index
Description
Format
G69
2
Dual slide/turret off
05. G-Group (modal)
G94
1
Linear feedrate in [mm/min, inch/min]
G95
2
Revolutional feedrate in [mm/rev, inch/rev]
06. G-Group (modal)
G20
1
Input system inch
G21
2
Input system metric
07. G-Group (modal)
G40
1
Deselection of cutter radius compensation
G41
2
Compensation left of contour
G42
3
Offset to right of contour
08. G-Group (modal)
10. G-Group (modal)
G80
1
Drilling cycle off
G80;
G83 2 Front face deep hole drilling G83 X(U)... C(H)... Z(W)... R... Q... P...
F... M... ;
G84 3 Front face tapping G84 X(U)... C(H)... Z(W)... R... P... F...
M... K... ;
G85 4 Front face drilling cycle G85 X(U)... C(H)... Z(W)... R... P... F...
K... M... ;
G87 5 Side surface deep hole drilling G87 Z(W)... C(H)... X(U)... R... Q... P...
F... M... ;
G88 6 Side surface tapping G88 Z(W)... C(H)... X(U)... R... P... F...
M... K... ;
G89 7 Side drilling G89 Z(W)... C(H)... X(U)... R... P... F...
K... M... ;
11. G-Group (modal)
G98
1
Return to starting point in drilling cycles
G99
2
Return to point R in drilling cycles
12. G-Group (modal)
G66
1
Macro module call
G66 P... L... <Parameters>;
G67
2
Delete macro-modal call
G67 P... L... <Parameters>;
14. G-Group (modal)
G54
1
Selecting work offset
G55 2 Selecting work offset
G56
3
Selecting work offset
G57 4 Selecting work offset
G58
5
Selecting work offset
G59
6
Selecting work offset
16. G-Group (modal)
G17
1
XY plane
G18
2
ZX plane
G19
3
YZ plane
18. G-Group (non-modal)
G4
1
Dwell time in [s] or spindle revolutions
G04 X...; or G04 P...;
G10
2
Write work offset/tool offset
G10 L2 Pp X... Z... ;
G28
3
1. Reference point approach
G28 X... Z... ;

Programming and Operating Manual (ISO Turning/Milling)
18 01/2017
Name
Index
Description
Format
G30
4
2./3./4. Reference point approach
G30 Pn X... Z... ;
G31
5
Delete measuring with distance-to-go
G31 X... Y... Z... F_;
G52
6
Programmable work offset
G65
7
Macro call
G65 P_ L_ ;
G70
8
Finishing cycle
G70 P... Q... ;
G71
9
Stock removal cycle, longitudinal axis
G71 U... R... ;
G72
10
Stock removal cycle, transverse axis
G72 W... R... ;
G73
11
Closed cutting cycle
G73 U... W... R... ;
G74
12
Multiple repetitive grooving cycles in the longitudinal axis
G74 R... ;
G75 13 Multiple repetitive grooving cycles in the transverse axis G75 R... ; or G75 X(U)... Z(W)... P...
Q... R... F... ;
G76
14
Multiple thread cutting cycle
G76 P... (m, r, a) Q... R... ;
G92
15
Set actual value
G92 (G50) X... Z... ;
G27
16
Referencing check (under development)
G27 X... Z... ;
G53 17 Approach position in machine coordinate system (G90) G53 X... Z... ;
G07.1 18 Cylindrical interpolation G07.1 A (B, C) r ;
G07.1 A (B, C) 0 ;
G5
20
High-speed cycle cutting
G05 Pxxxxx Lxxx ;
G30.1
21
Reference point position
G5.1
22
High-speed cycle -> Call of CYCLE305
G92.1
23
Delete actual value, reset the WCS
G60
24
directed positioning
21. G-Group (modal)
G13.1
1)
1
TRANSMIT OFF
G12.1
2
TRANSMIT ON
31. G-Group (modal)
G290
1
Select Siemens mode
G291
2
Select ISO dialect mode
3.1.3
SINUMERIK ISO dialect turning mode C
Name
Index
Description
Format
01. G-Group (modal)
G0
1
Rapid traverse
G00 X... Y... Z... ;
G1
2
Linear motion
G01 X... Z... F... ;
G2
3
Circle/helix in clockwise direction
G02(G03) X(U)... Z(W)... I... K... (R...)
F... ;
G3
4
Circle/helix in counterclockwise direction
G33
5
Thread cutting with constant lead
G33 X (U)... Z (W)... F... ;
G20
6
Longitudinal turning cycle
G... X... Z... R... F... ;
G21
7
Thread cutting cycle
G... X... Z... F... ;
G24
8
Face turning cycle
G... X... Z... F... ;
G34
9
Thread cutting with variable lead
G34 X (U)... Z (W)... F... K... ;
02. G-Group (modal)
G96
1
Constant cutting rate on
G96 S...
G97
2
Constant cutting rate off
G97 S...
03. G-Group (modal)
G90
1
Absolute programming

Programming and Operating Manual (ISO Turning/Milling)
01/2017 19
Name
Index
Description
Format
G91
2
Incremental programming
04. G-Group (modal)
G68
1
Dual slide/turret on
G69
2
Dual slide/turret off
05. G-Group (modal)
G94
1
Linear feedrate in [mm/min, inch/min]
G95
2
Revolutional feedrate in [mm/rev, inch/rev]
06. G-Group (modal)
G70
1
Input system inch
G70 P... Q... ;
G71
2
Input system metric
G71 U... R... ;
07. G-Group (modal)
G40
1
Deselection of cutter radius compensation
G41
2
Compensation left of contour
G42
3
Offset to right of contour
08. G-Group (modal)
10. G-Group (modal)
G80
1
Drilling cycle off
G80;
G83 2 Front face deep hole drilling G83 X(U)... C(H)... Z(W)... R... Q... P...
F... M... ;
G84 3 Front face tapping G84 X(U)... C(H)... Z(W)... R... P... F...
M... K... ;
G85 4 Front face drilling cycle G85 X(U)... C(H)... Z(W)... R... P... F...
K... M... ;
G87 5 Side surface deep hole drilling G87 Z(W)... C(H)... X(U)... R... Q... P...
F... M... ;
G88 6 Side surface tapping G88 Z(W)... C(H)... X(U)... R... P... F...
M... K... ;
G89 7 Side drilling G89 Z(W)... C(H)... X(U)... R... P... F...
K... M... ;
11. G-Group (modal)
G98
1
Return to starting point in drilling cycles
G99
2
Return to point R in drilling cycles
12. G-Group (modal)
G66
1
Macro module call
G66 P... L... <Parameters>;
G67 2 Delete macro-modal call G67 P... L... <Parameters>;
14. G-Group (modal)
G54 1 Selecting work offset
G55
2
Selecting work offset
G56
3
Selecting work offset
G57
4
Selecting work offset
G58
5
Selecting work offset
G59
6
Selecting work offset
16. G-Group (modal)
G17
1
XY plane
G18
2
ZX plane
G19
3
YZ plane
18. G-Group (non-modal)

Programming and Operating Manual (ISO Turning/Milling)
20 01/2017
Name
Index
Description
Format
G4
1
Dwell time in [s] or spindle revolutions
G04 X...; or G04 P...;
G10
2
Write work offset/tool offset
G10 L2 Pp X... Z... ;
G28
3
1. Reference point approach
G28 X... Z... ;
G30
4
2./3./4. Reference point approach
G30 Pn X... Z... ;
G31
5
Delete measuring with distance-to-go
G31 X... Y... Z... F_;
G52
6
Programmable work offset
G65
7
Macro call
G65 P_ L_ ;
G72
8
Finishing cycle
G72 P... Q... ;
G73
9
Stock removal cycle, longitudinal axis
G73 U... R... ;
G74
10
Stock removal cycle, transverse axis
G74 W... R... ;
G75
11
Contour repetition
G75 U... W... R... ;
G76
12
Multiple repetitive grooving cycles in the longitudinal axis
G76 R... ;
G77 13 Multiple repetitive grooving cycles in the transverse axis G77 R... ; or G77 X(U)... Z(W)... P...
Q... R... F... ;
G78 14 Multiple thread cutting cycle G78 P... (m, r, a) Q... R... ;
G92
15
Set actual value
G92 (G50) X... Z... ;
G27
16
Referencing check (under development)
G27 X... Z... ;
G53
17
Approach position in machine coordinate system
(G90) G53 X... Z... ;
G07.1 18 Cylindrical interpolation G07.1 A (B, C) r ;
G07.1 A (B, C) 0 ;
G5
20
High-speed cycle cutting
G05 Pxxxxx Lxxx ;
G30.1
21
Reference point position
G5.1
22
High-speed cycle -> Call of CYCLE305
G92.1
23
Delete actual value, reset the WCS
G60
24
directed positioning
21. G-Group (modal)
G13.1
1)
1
TRANSMIT OFF
G12.1
2
TRANSMIT ON
31. G-Group (modal)
G290
1
Select Siemens mode
G291
2
Select ISO dialect mode
3.2
Travel commands
3.2.1
Interpolation commands
The positioning and interpolation commands, with which the tool path along the programmed contour, such as a straight line
or a circular arc, is monitored, are described in the next Section.
3.2.1.1
Rapid traverse (G00)
You can use the rapid traverse movements to position the tool rapidly, to travel around the workpiece or to approach tool
change points.
The following G functions can be used for positioning:
G function
Function
G group
G00
Rapid traverse
01
G01
Linear motion
01
G02
Circle/helix in clockwise direction
01