Siemens SINUMERIK 808D User manual

Turning Part 2: Programming

(Siemens instructions)
_
_________________
_
_
_________________
_
_
_________________
_
SINUMERIK
SINUMERIK 808D
Turning Part 2: Programming
(Siemens instructions)
Programming and Operating Manual
Valid for:
SINUMERIK 808D Turning (software version: V4.4)
Target group:
End users and service engineers
05/2012
6FC5398-5DP10-0BA0
Programming principles
1
Cycles
2
Typical turning program
3

Legal information
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
with a safety alert symbol, indicates that minor personal injury can result if proper precautions are not taken.
CAUTION
without a safety alert symbol, indicates that property damage can result if proper precautions are not taken.
NOTICE
indicates that an unintended result or situation can occur if the relevant information is not taken into account.
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.
Trademarks
All names identified by ® are registered trademarks of Siemens AG. The remaining trademarks in this publication
may be trademarks whose use by third parties for their own purposes could violate the rights of the owner.
Disclaimer of Liability
We have reviewed the contents of this publication to ensure consistency with the hardware and software
described. Since variance cannot be precluded entirely, we cannot guarantee full consistency. However, the
information in this publication is reviewed regularly and any necessary corrections are included in subsequent
editions.
Siemens AG
Industry Sector
Postfach 48 48
90026 NÜRNBERG
GERMANY
Order number: 6FC5398-5DP10-0BA0
Ⓟ 06/2012 Technical data subject to change
Copyright © Siemens AG 2012.
All rights reserved

Turning Part 2: Programming (Siemens instructions)
Programming and Operating Manual, 05/2012, 6FC5398-5DP10-0BA0 3
Table of contents
1 Programming principles ............................................................................................................................. 7
1.1 Fundamentals of programming......................................................................................................7
1.1.1 Program names .............................................................................................................................7
1.1.2 Program structure ..........................................................................................................................7
1.1.3 Word structure and address...........................................................................................................8
1.1.4 Character set..................................................................................................................................9
1.1.5 Block format .................................................................................................................................10
1.1.6 List of instructions ........................................................................................................................12
1.2 Positional data .............................................................................................................................25
1.2.1 Programming dimensions ............................................................................................................25
1.2.2 Absolute / incremental dimensioning: G90, G91, AC, IC.............................................................26
1.2.3 Dimensions in metric units and inches: G71, G70, G710, G700.................................................28
1.2.4 Radius / diameter dimensions: DIAMOF, DIAMON, DIAM90......................................................29
1.2.5 Programmable work offset: TRANS, ATRANS ............................................................................30
1.2.6 Programmable scaling factor: SCALE, ASCALE.........................................................................33
1.2.7 Workpiece clamping - settable work offset: G54 to G59, G500, G53, G153...............................34
1.3 Axis movements...........................................................................................................................35
1.3.1 Linear interpolation with rapid traverse: G0.................................................................................35
1.3.2 Feedrate F....................................................................................................................................36
1.3.3 Linear interpolation with feedrate: G1..........................................................................................37
1.3.4 Circular interpolation: G2, G3 ......................................................................................................38
1.3.5 Circular interpolation via intermediate point: CIP.........................................................................41
1.3.6 Circle with tangential transition: CT .............................................................................................42
1.3.7 Thread cutting with constant lead: G33 .......................................................................................42
1.3.8 Programmable run-in and run-out path for G33: DITS, DITE......................................................45
1.3.9 Thread cutting with variable lead: G34, G35 ...............................................................................46
1.3.10 Thread interpolation: G331, G332 ...............................................................................................48
1.3.11 Fixed point approach: G75...........................................................................................................49
1.3.12 Reference point approach: G74...................................................................................................50
1.3.13 Exact stop / continuous-path control mode: G9, G60, G64 .........................................................50
1.3.14 Acceleration pattern: BRISK, SOFT.............................................................................................53
1.3.15 The third axis................................................................................................................................54
1.3.16 Dwell Time: G4.............................................................................................................................55
1.4 Spindle movements .....................................................................................................................56
1.4.1 Spindle speed S, directions of rotation ........................................................................................56
1.4.2 Spindle positioning.......................................................................................................................57
1.4.2.1 Spindle positioning (SPOS, SPOSA, M19, M70, WAITS) ...........................................................57
1.4.2.2 Spindle positioning (SPOS, SPOSA, M19, M70, WAITS): Further information...........................63
1.4.3 Gear stages..................................................................................................................................64
1.5 Special turning functions..............................................................................................................65
1.5.1 Constant cutting rate: G96, G97 ..................................................................................................65
1.5.2 Rounding, chamfer.......................................................................................................................67
1.5.3 Contour definition programming...................................................................................................70

Table of contents
Turning Part 2: Programming (Siemens instructions)
4 Programming and Operating Manual, 05/2012, 6FC5398-5DP10-0BA0
1.6 Tool and tool offset...................................................................................................................... 72
1.6.1 General information (turning) ...................................................................................................... 72
1.6.2 Tool T (turning)............................................................................................................................ 72
1.6.3 Tool offset number D (turning) .................................................................................................... 73
1.6.4 Selecting the tool radius compensation: G41, G42 .................................................................... 77
1.6.5 Corner behavior: G450, G451..................................................................................................... 79
1.6.6 Tool radius compensation OFF: G40.......................................................................................... 80
1.6.7 Special cases of the tool radius compensation........................................................................... 81
1.6.8 Example of tool radius compensation (turning)........................................................................... 82
1.6.9 Special handling of tool compensation (turning)......................................................................... 83
1.7 Miscellaneous function M............................................................................................................ 84
1.8 H function .................................................................................................................................... 85
1.9 Arithmetic parameters, LUD and PLC variables ......................................................................... 85
1.9.1 Arithmetic parameter R ............................................................................................................... 85
1.9.2 Local User Data (LUD)................................................................................................................ 87
1.9.3 Reading and writing PLC variables............................................................................................. 89
1.10 Program jumps............................................................................................................................ 90
1.10.1 Unconditional program jumps ..................................................................................................... 90
1.10.2 Conditional program jumps ......................................................................................................... 91
1.10.3 Program example for jumps........................................................................................................ 93
1.10.4 Jump destination for program jumps........................................................................................... 94
1.11 Subroutine technique .................................................................................................................. 94
1.11.1 General information..................................................................................................................... 94
1.11.2 Calling machining cycles (turning) .............................................................................................. 97
1.11.3 Executing external subroutines (EXTCALL) ............................................................................... 97
1.12 Timers and workpiece counters .................................................................................................. 99
1.12.1 Runtime timer.............................................................................................................................. 99
1.12.2 Workpiece counter .................................................................................................................... 101
2 Cycles.................................................................................................................................................... 103
2.1 Overview of cycles .................................................................................................................... 103
2.2 Programming cycles.................................................................................................................. 106
2.3 Graphical cycle support in the program editor .......................................................................... 107
2.4 Drilling cycles ............................................................................................................................ 108
2.4.1 General information................................................................................................................... 108
2.4.2 Requirements............................................................................................................................ 109
2.4.3 Drilling, centering - CYCLE81 ................................................................................................... 112
2.4.4 Drilling, counterboring - CYCLE82............................................................................................ 115
2.4.5 Deep-hole drilling - CYCLE83................................................................................................... 118
2.4.6 Rigid tapping - CYCLE84.......................................................................................................... 123
2.4.7 Tapping with compensating chuck - CYCLE840....................................................................... 128
2.4.8 Reaming1 - CYCLE85............................................................................................................... 133
2.4.9 Boring - CYCLE86..................................................................................................................... 135
2.4.10 Boring with stop 1- CYCLE87 ................................................................................................... 138
2.4.11 Drilling with stop 2 - CYCLE88.................................................................................................. 140
2.4.12 Reaming 2 - CYCLE89.............................................................................................................. 142
2.5 Turning cycles ........................................................................................................................... 144

Table of contents
Turning Part 2: Programming (Siemens instructions)
Programming and Operating Manual, 05/2012, 6FC5398-5DP10-0BA0 5
2.5.1 Requirements.............................................................................................................................144
2.5.2 Cutoff - CYCLE92 ......................................................................................................................146
2.5.3 Groove - CYCLE93 ....................................................................................................................148
2.5.4 Undercut (forms E and F to DIN) - CYCLE94............................................................................157
2.5.5 Cutting with relief cut - CYCLE95 ..............................................................................................161
2.5.6 Thread undercut - CYCLE96 .....................................................................................................177
2.5.7 Thread chaining - CYCLE98......................................................................................................181
2.5.8 Thread cutting - CYCLE99.........................................................................................................187
2.6 Error messages and error handling ...........................................................................................195
2.6.1 General Information ...................................................................................................................195
2.6.2 Error handling in the cycles........................................................................................................195
2.6.3 Overview of cycle alarms ...........................................................................................................195
2.6.4 Messages in the cycles..............................................................................................................196
3 Typical turning program ......................................................................................................................... 197
Index...................................................................................................................................................... 207

Table of contents
Turning Part 2: Programming (Siemens instructions)
6 Programming and Operating Manual, 05/2012, 6FC5398-5DP10-0BA0

Turning Part 2: Programming (Siemens instructions)
Programming and Operating Manual, 05/2012, 6FC5398-5DP10-0BA0 7
Programming principles 1
1.1 Fundamentals of programming
1.1.1 Program names
Each program must have a program name. The program name must follow the conventions
below:
● Use only English letters or numbers for a program name, if the user interface language is
English; use only Chinese letters or numbers for a program name, if the user interface
language is Chinese.
● Separate the file extension of a subprogram name only with a decimal point
● Use a maximum of 24 English characters or of 12 Chinese characters for a program
name
NOTICE
It is not recommended that you use a special character for the first character of a
program name.
When you create a new main program, it is not necessary to enter the file extension
".MPF". When you desire to create a subprogram, you must enter the file extension
".SPF".
Examples
WORKPIECE527
1.1.2 Program structure
Structure and content
The NC program consists of a sequence of blocks (see the table below). Each block
represents a machining step. Instructions are written in the blocks in the form of words. The
last block in the execution sequence contains a special word for the end of the program, for
example, M2.
The table below shows you an example of the NC program structure.
Block Word Word Word ... ; Comment
Block N10 G0 X20 ... ; First block
Block N20 G2 Z37 ... ; Second block
Block N30 G91 ... ... ; ...
Block N40 ... ... ...
Block N50 M2 ; End of program

Programming principles
1.1 Fundamentals of programming
Turning Part 2: Programming (Siemens instructions)
8 Programming and Operating Manual, 05/2012, 6FC5398-5DP10-0BA0
1.1.3 Word structure and address
Functionality/structure
A word is a block element and mainly constitutes a control command. The word consists of
the following two parts:
● address character: generally a letter
● numerical value: a sequence of digits which with certain addresses can be added by a
sign put in front of the address, and a decimal point.
A positive sign (+) can be omitted.
The following picture shows an example of the word structure.
:RUG :RUG :RUG
$GGUHVV 9DOXH $GGUHVV 9DOXH $GGUHVV 9DOXH
([DPSOH
([DPSOH
([SODQDWLRQ
([SODQDWLRQ
*
*
;
;
)
)
7UDYHUVHZLWK
/LQHDU
LQWHUSRODWLRQ
3DWKRUHQG
SRVLWLRQIRUWKH
;D[LVPP
)HHGUDWH
PPPLQ
Several address characters
A word can also contain several address letters. In this case, however, the numerical value
must be assigned via the intermediate character "=".
Example: CR=5.23
Additionally, it is also possible to call G functions using a symbolic name (For more
information, refer to the topic "List of instructions (Page 12)".).
Example: SCALE ; Enable scaling factor
Extended address
With the following addresses, the address is extended by 1 to 4 digits to obtain a higher
number of addresses. In this case, the value must be assigned using an equality sign "=".
R Arithmetic parameters
H H function
I, J, K Interpolation parameters/intermediate point
M Special function M, affecting the spindle with other options
S Spindle speed
Examples: R10=6.234 H5=12.1 I1=32.67 M2=5 S1=400

Programming principles
1.1 Fundamentals of programming
Turning Part 2: Programming (Siemens instructions)
Programming and Operating Manual, 05/2012, 6FC5398-5DP10-0BA0 9
1.1.4 Character set
The following characters are used for programming. They are interpreted in accordance with
the relevant definitions.
Letters, digits
A, B, C, D, E, F, G, H, I, J, K, L, M, N,O, P, Q, R, S, T, U, V, W X, Y, Z
0, 1, 2, 3, 4, 5, 6, 7, 8, 9
No distinction is made between lowercase and uppercase letters.
Printable special characters
( Open parenthesis " Inverted commas
) Close parenthesis _ Underscore (belongs to letters)
[ Open square bracket . Decimal point
] Close square bracket , Comma, separator
< less than ; Comment start
> greater than % Reserved; do not use
: Main block, end of label & Reserved; do not use
= Assignment, part of equation ' Reserved; do not use
/ skip $ System variable identifiers
* Multiplication ? Reserved; do not use
+ Addition and positive sign ! Reserved; do not use
- Subtraction, minus sign
Non-printable special characters
LF End-of-block character
Blank Separator between words; blank
Tab character Reserved; do not use

Programming principles
1.1 Fundamentals of programming
Turning Part 2: Programming (Siemens instructions)
10 Programming and Operating Manual, 05/2012, 6FC5398-5DP10-0BA0
1.1.5 Block format
Functionality
A block should contain all data required to execute a machining step.
Generally, a block consists of several words and is always completed with the
end-of-block character " LF " (Linefeed). This character is automatically generated when
pressing the linefeed or <INPUT> key when writing.
1 :RUG :RUG  :RUGQ &RPPHQW /)
6SDFH
%/$1.
6SDFH

6SDFH

6SDFH

%ORFNLQVWUXFWLRQV
%ORFNQXPEHUVWDQGVLQIURQWRILQVWUXFWLRQV
2QO\DVQHHGHGLQVWHDGRI1PDLQEORFNVKDYH
WKHV\PEROಯಯ&RORQ
%ORFNVNLS
RQO\LIQHFHVVDU\VWDQGVDWWKHEHJLQQLQJ
(QGRIEORFNFKDUDFWHU
RQO\LIUHTXLUHG
LVZULWWHQDWWKHHQGGHOLPLWHGIURP
WKHUHPDLQLQJSDUWRIWKHEORFNE\
7RWDOQXPEHURIFKDUDFWHUVLQDEORFNFKDUDFWHUV
Figure 1-1 block structure diagram
Word order
If there are several instructions in a block, the following order is recommended:
N... G... X... Z... F... S... T... D... M... H...
Note regarding block numbers
First select the block numbers in steps of 5 or 10. Thus, you can later insert blocks and
nevertheless observe the ascending order of block numbers.
Block skip
Blocks of a program, which are to be executed not with each program run, can be marked by
a slash / in front of the block number.
The block skip itself is activated via Operation (program control: "SKP") or by the
programmable controller (signal). A section can be skipped by several blocks in succession
using " / ".
If a block must be skipped during program execution, all program blocks marked with " / " are
not executed. All instructions contained in the blocks concerned will not be considered. The
program is continued with the next block without marking.

Programming principles
1.1 Fundamentals of programming
Turning Part 2: Programming (Siemens instructions)
Programming and Operating Manual, 05/2012, 6FC5398-5DP10-0BA0 11
Comment, remark
The instructions in the blocks of a program can be explained using comments (remarks). A
comment always starts with a semicolon " ; " and ends with end-of-block.
Comments are displayed together with the contents of the remaining block in the current
block display.
Messages
Messages are programmed in a separate block. A message is displayed in a special field
and remains active until a block with a new message is executed or until the end of the
program is reached. Max. 65 characters can be displayed in message texts.
A message without message text cancels a previous message.
MSG("THIS IS THE MESSAGE TEXT")
Programming example
N10 ; G&S company, order no. 12A71
N20 ; Pump part 17, drawing no.: 123 677
N30 ; Program created by H. Adam, Dept. TV 4
N40 MSG("DRAWING NO.: 123677")
:50 G54 F4.7 S220 D2 M3 ;Main block
N60 G0 G90 X100 Z200
N70 G1 Z185.6
N80 X112
/N90 X118 Z180 ; Block can be suppressed
N100 X118 Z120
N110 G0 G90 X200
N120 M2 ; End of program

Programming principles
1.1 Fundamentals of programming
Turning Part 2: Programming (Siemens instructions)
12 Programming and Operating Manual, 05/2012, 6FC5398-5DP10-0BA0
1.1.6 List of instructions
The functions marked with an asterisk (*) are active at the start of the program in the CNC
turning version, unless otherwise programmed or the machine manufacturer has preserved
the default setting for the "turning" technology.
Address Significance Value assignments Information Programming
D Tool offset number 0 ... 9, only integer, no
sign
Contains compensation data for
a particular tool T... ; D0-
>compensation values= 0,
max. 9 D numbers for one tool
D...
F Feedrate 0.001 ... 99 999.999 Path velocity of a
tool/workpiece;
unit: mm/min or mm/revolution
depending on G94 or G95
F...
F Dwell time (block
with G4)
0.001 ... 99 999.999 Dwell time in seconds G4 F...; separate block
F Thread lead
change (block
containing G34,
G35)
0.001 ... 99 999.999 in mm/rev2 See G34, G35
G G function
(preparatory
function)
Only integer, specified
values
The G functions are divided into
G groups. Only one G function
of a group can be programmed
in a block.
A G function can be either
modal (until it is canceled by
another function of the same
group) or only effective for the
block in which it is programmed
(non-modal).
G...
or symbolic name, e.g.:
CIP
G group:
G0 Linear interpolation at rapid traverse rate 1: Motion commands G0 X... Z...
G1 * Linear interpolation at feedrate (type of interpolation) G1 X...Z... F...
G2 Circular interpolation clockwise G2 X... Z... I... K... F...
;Center and end point
G2 X... Z... CR=... F...
;Radius and end point
G2 AR=... I... K... F...
;opening angle and
center point
G2 AR=... X... Z... F...
;opening angle and end
point
G3 Circular interpolation counter-clockwise G3 ... ; otherwise as for
G2
CIP Circular interpolation through intermediate
point
CIP X... Z... I1=... K1=...
F... ;I1, K1 is intermediate
point

Programming principles
1.1 Fundamentals of programming
Turning Part 2: Programming (Siemens instructions)
Programming and Operating Manual, 05/2012, 6FC5398-5DP10-0BA0 13
Address Significance Value assignments Information Programming
CT Circular interpolation; tangential transition N10 ...
N20 CT Z... X... F...
;circle, tangential
transition
to the previous path
segment N10
G33 Thread cutting with constant lead modally effective ;Constant lead
G33 Z... K... SF=... ;
cylindrical thread
G33 X... I... SF=... ; face
thread
G33 Z... X... K... SF=... ;
taper thread, in Z axis
path larger than in the X
axis
G33 Z... X... I... SF=... ;
taper thread, in X axis
path larger than in the Z
axis
G34 Thread cutting, increasing lead G33 Z... K... SF=... ;
cylindrical thread,
constant lead
G34 Z... K... F17.123 ;
lead increasing with
; 17.123 mm/rev2
G35 Thread cutting, decreasing lead G33 Z... K... SF=... ;
cylindrical lead
G35 Z... K... F7.321 ;
lead decreasing with
; 7.321 mm/rev2
G331 Thread interpolation N10 SPOS=... ; Spindle
in position control
N20 G331 Z... K... S... ;
tapping without
compensating chuck e.g.
in Z axis
; RH or LH thread is
defined via the sign of the
lead (e.g. K+): + : as with
M3
- : as with M4
G332 Thread interpolation - retraction G332 Z... K... ;tapping
without compensating
chuck, e.g. in Z axis,
retraction motion
; sign of lead as for G331
G4 Dwell time 2: Special motions, dwell time
non-modal
G4 F...;separate block, F:
Time in seconds
or
G4 S.... ;separate block,
S: in spindle revolutions

Programming principles
1.1 Fundamentals of programming
Turning Part 2: Programming (Siemens instructions)
14 Programming and Operating Manual, 05/2012, 6FC5398-5DP10-0BA0
Address Significance Value assignments Information Programming
G74 Reference point approach G74 X1=0 Z1=0
;separate block,
(machine axis identifier!)
G75 Fixed point approach G75 X1=0 Z1=0
;separate block,
(machine axis identifier!)
TRANS translation, programmable 3: Write memory TRANS X... Z... ;separate
block
SCALE Programmable scaling factor non-modal SCALE X... Z... ; scaling
factor in the direction
of the specified axis,
separate block
ROT rotation, programmable ROT RPL=... ;rotation in
the current plane
G17 to G19, separate
block
MIRROR Programmable mirroring MIRROR X0 ; coordinate
axis whose
direction is changed,
separate block
ATRANS additive translation, programming ATRANS X... Z... ;
separate block
ASCALE Additive programmable scaling factor ASCALE X... Z... ; scaling
factor in the direction
of the specified axis,
separate block
AROT additive programmable rotation AROT RPL=... ; rotation
in the current plane
G17 to G19,
separate block
AMIRROR additive programmable mirroring AMIRROR X0 ;
coordinate axis whose
direction is changed,
separate block
G17 X/Y plane (when center-drilling required) 6: Plane selection
G18 * Z/X plane (standard turning)
G19 Y/Z plane
G40 * Tool radius compensation OFF
G41 Tool radius compensation left of contour
G42 Tool radius compensation right of contour
7: Tool radius compensation
modally effective
G500 * Settable work offset OFF
G54 1. Settable work offset
G55 2. settable work offset
G56 3. settable work offset
G57 4. settable work offset
8: Settable work offset
modally effective
G58 5. settable work offset
G59 6. settable work offset

Programming principles
1.1 Fundamentals of programming
Turning Part 2: Programming (Siemens instructions)
Programming and Operating Manual, 05/2012, 6FC5398-5DP10-0BA0 15
Address Significance Value assignments Information Programming
G53 Non-modal skipping of the settable work
offset
9: Suppressing the settable work
offset
non-modal
G153 Non-modal skipping of the settable work
offset including base frame
G60 * Exact stop
G64 Continuous-path mode
10: Approach behavior
modally effective
G62 Corner deceleration at inside corners when
tool radius offset is active (G41, G42)
Only in conjunction with
continuous-path mode.
G62 Z... G1
G9 Non-modal exact stop 11: Non-modal exact stop
non-modal
G601 * Exact stop window, fine, with G60, G9
G602 Exact stop window, coarse, with G60, G9
12: Exact stop window
modally effective
G621 Corner deceleration at all corners Only in conjunction with
continuous-path mode.
G621 AIDS=...
G70 Inch dimension input
G71 * Metric dimension data input
13: Inch/metric dimension data
modally effective
G700 Inch dimension data input; also for feedrate
F
G710 Metric dimension data input; also for
feedrate F
G90 * Absolute dimension data input
G91 Incremental dimension input
14: Absolute / incremental
dimension
modally effective
G94 Feed F in mm/min
G95 * Feedrate F in mm/spindle revolutions
G96 Constant cutting rate ON
(F in mm/rev., S in m/min)
G96 S... LIMS=... F...
G97 Constant cutting speed OFF
15: Feedrate / spindle
modally effective
G450 * Transition circle
G451 Point of intersection
18: Behavior at corners when
working with tool radius
compensation
modally effective
BRISK * Jerking path acceleration
SOFT Jerk-limited path acceleration
21: Acceleration profile
modally effective
FFWOF * Feedforward control OFF
FFWON Feedforward control ON
24: Feedforward control
modally effective
DIAMOF Radius dimensioning
DIAMON * Diameter dimensioning
29: Dimension Radius / diameter
modally effective
G290 * SIEMENS mode
G291 External mode
47: External NC languages
modally effective

Programming principles
1.1 Fundamentals of programming
Turning Part 2: Programming (Siemens instructions)
16 Programming and Operating Manual, 05/2012, 6FC5398-5DP10-0BA0
Address Significance Value assignments Information Programming
H
H0=
to
H9999=
H function ± 0.0000001 ...
9999 9999
(8 decimal places) or
specified as an
exponent:
± (10-300 ... 10+300 )
Value transfer to the PLC;
significance defined by the
machine manufacturer
H0=... H9999=...
e.g.: H7=23.456
I Interpolation
parameters
±0.001 ... 99 999.999
Thread:
0.001 ... 2000.000
Belongs to the X axis; meaning
dependent on G2,G3 ->circle
center or
G33, G34, G35 G331, G332 ->
thread lead
See G2, G3 and G33,
G34, G35
K Interpolation
parameters
±0.001 ... 99 999.999
Thread:
0.001 ... 2000.000
Belongs to the Z axis; otherwise,
as with I
See G2, G3 and G33,
G34, G35
I1= Intermediate point
for circular
interpolation
±0.001 ... 99 999.999 Belongs to the X axis;
specification for circular
interpolation with CIP
See CIP
K1= Intermediate point
for circular
interpolation
±0.001 ... 99 999.999 Belongs to the Z axis;
specification for circular
interpolation with CIP
See CIP
L Subroutine; name
and call
7 decimals;
integer only, no sign
Instead of a free name, it is also
possible to select L1
...L9999999;
this also calls the subroutine
(UP) in a separate block,
Please note: L0001 is not
always equal to L1.
The name "LL6" is reserved for
the tool change subroutine.
L.... ;separate block
M Additional function 0 ... 99
only integer, no sign
For example, for initiating
switching actions,
such as "coolant ON",
maximum five M functions per
block.
M...
M0 Programmed stop The machining is stopped at the
end of a block containing M0; to
continue, press NC START.
M1 Optional stop As with M0, but the stop is only
performed if a special signal
(Program control: "M01") is
present.
M2 End of main program with return to
beginning of program
Can be found in the last block of
the processing sequence
M30 End of program (as M2) Can be found in the last block of
the processing sequence
M17 End of subroutine Can be found in the last block of
the processing sequence
M3 CW rotation of spindle
M4 CCW rotation of spindle
M5 Spindle stop

Programming principles
1.1 Fundamentals of programming
Turning Part 2: Programming (Siemens instructions)
Programming and Operating Manual, 05/2012, 6FC5398-5DP10-0BA0 17
Address Significance Value assignments Information Programming
Mn=3 CW rotation of spindle n = 1 M1=3 ; CW rotation stop
for spindle 1
Mn=4 CCW rotation of spindle (for spindle n) n = 1 M1=4 ; CCW rotation
stop for spindle 1
Mn=5 Spindle stop (for spindle n) n = 1 M1=5 ; Spindle stop for
spindle 1
M6 Tool change Only if activated with M6 via the
machine control panel;
otherwise, change directly using
the T command
M40 Automatic gear stage switching
Mn=40 Automatic gear stage switching
(for spindle n)
n = 1 M1=40 ; automatic gear
stage; for spindle 1
M41 to M45 Gear stage 1 to gear stage 5
Mn=41 to
Mn=45
Gear stage 1 to gear stage 5 (for spindle n) n = 1 M1=41; 1st gear stage for
spindle 1
M70, M19 - Reserved; do not use
M... Remaining M functions Functionality is not defined by
the control system and can
therefore be used freely by the
machine manufacturer
N Block number -
subblock
0 ... 9999 9999
only integer, no sign
Can be used to identify blocks
with a number; is written at the
beginning of a block.
N20
: Block number of a
main block
0 ... 9999 9999
only integer, no sign
Special block identification, used
instead of N... ; such a block
should contain all instructions for
a complete subsequent
machining step.
:20
P Number of
subroutine passes
1 ... 9999
only integer, no sign
Is used if the subroutine is run
several times and is contained in
the same block as the call
L781 P... ;separate block
N10 L871 P3 ; three
cycles
R0
to
R299
Arithmetic
parameters
± 0.0000001 ...
9999 9999
(8 decimal places) or
specified as an
exponent:
± (10-300 ... 10+300 )
R1=7.9431 R2=4
with specification of an
exponent:
R1=-1.9876EX9; R1=-1
987 600 000
Arithmetic functions In addition to the 4 basic
arithmetic functions using the
operands + - * /, there are the
following arithmetic functions:
SIN( ) Sine Degrees R1=SIN(17.35)
COS() Cosine Degrees R2=COS(R3)
TAN() Tangent Degrees R4=TAN(R5)
ASIN() Arc sine R10=ASIN(0.35) ; R10:
20.487 degrees

Programming principles
1.1 Fundamentals of programming
Turning Part 2: Programming (Siemens instructions)
18 Programming and Operating Manual, 05/2012, 6FC5398-5DP10-0BA0
Address Significance Value assignments Information Programming
ACOS() Arc cosine R20=ACOS(R2) ; R20: ...
Degrees
ATAN2( , ) Arctangent2 The angle of the sum vector is
calculated from 2 vectors
standing vertically one on
another. The 2nd vector
specified is always used for
angle reference.
Result in the range: -180 to
+180 degrees
R40=ATAN2(30.5,80.1) ;
R40: 20.8455 degrees
SQRT() Square root R6=SQRT(R7)
POT() Square R12=POT(R13)
ABS() Absolute value R8=ABS(R9)
TRUNC() Truncate to integer R10=TRUNC(R2)
LN() Natural logarithm R12=LN(R9)
EXP() Exponential
function
R13=EXP(R1)
RET Subroutine end Used instead of M2 - to maintain
the continuous-path mode
RET ;separate block
S... Spindle speed 0.001 ... 99 999.999 Unit of measurement of the
spindle r.p.m.
S...
S1=... Spindle speed
for spindle 1
0.001 ... 99 999.999 Unit of measurement of the
spindle r.p.m.
S1=725 ; speed 725
r.p.m. for spindle 1
S Cutting rate
with G96 active
0.001 ... 99 999.999 Cutting rate unit m/min with
G96; for spindle only
G96
S...
S Dwell time
in block with G4
0.001 ... 99 999.999 Dwell time in spindle revolutions G4 S... ;separate block
T Tool number 1 ... 32 000
only integer, no sign
The tool change can be
performed either directly using
the T command or only with M6.
This can be set in the machine
data.
T...
X Axis ±0.001 ... 99 999.999 Positional data X...
Y Axis ±0.001 ... 99 999.999 Positional data Y...
Z Axis ±0.001 ... 99 999.999 Positional data Z...
AC Absolute
coordinate
- The dimension can be specified
for the end or center point of a
certain axis, irrespective of G91.
N10 G91 X10 Z=AC(20)
;X -incremental
dimension,
Z - absolute dimension
ACC[ axis ] Percentage
acceleration
override
1 ... 200, integer Acceleration override for an axis
or spindle; specified as a
percentage
N10 ACC[X]=80 ;for the X
axis 80%
N20 ACC[S]=50;for the
spindle: 50%

Programming principles
1.1 Fundamentals of programming
Turning Part 2: Programming (Siemens instructions)
Programming and Operating Manual, 05/2012, 6FC5398-5DP10-0BA0 19
Address Significance Value assignments Information Programming
ACP Absolute
coordinate;
approach position
in the positive
direction
(for rotary axis,
spindle)
- It is also possible to specify the
dimensions for the end point of a
rotary axis with ACP(...)
irrespective of G90/G91; also
applies to spindle positioning
N10 A=ACP(45.3)
;approach absolute
position of the A axis in
the positive direction
N20 SPOS=ACP(33.1)
;position spindle
ACN Absolute
coordinate;
approach position
in the negative
direction
(for rotary axis,
spindle)
- It is also possible to specify the
dimensions for the end point of a
rotary axis with ACN(...)
irrespective of G90/G91; also
applies to spindle positioning
N10 A=ACN(45.3)
;approach absolute
position of the A axis in
the negative direction
N20 SPOS=ACN(33.1)
;position spindle
ANG Angle for the
specification of a
straight line for the
contour definition
±0.00001 ...
359.99999
Specified in degrees;
one possibility of specifying a
straight line when using G0 or
G1 if only one end-point
coordinate of the plane is known
or
if the complete end point is
known with contour ranging over
several blocks
N10 G1 X... Z....
N11 X... ANG=...
or contour over several
blocks:
N10 G1 X... Z...
N11 ANG=...
N12 X... Z... ANG=...
AR Aperture angle for
circular
interpolation
0.00001 ... 359.99999 Specified in degrees; one
possibility of defining the circle
when using G2/G3
See G2, G3
CALL Indirect cycle call - Special form of the cycle call; no
parameter transfer; the name of
the cycle is stored in a variable;
only intended for cycle-internal
use
N10 CALL VARNAME ;
variable name
CHF Chamfer;
general use
0.001 ... 99 999.999 Inserts a chamfer of the
specified chamfer length
between two contour blocks
N10 X... Z.... CHF=...
N11 X... Z...
CHR Chamfer;
in the contour
definition
0.001 ... 99 999.999 Inserts a chamfer of the
specified leg length between two
contour blocks
N10 X... Z.... CHR=...
N11 X... Z...
CR Radius for circular
interpolation
0.010 ... 99 999.999
Negative sign - for
selecting the circle:
greater than semicircle
One possibility of defining a
circle when using G2/G3
See G2, G3
CYCLE... Machining cycle Only specified values The call of the machining cycles
requires a separate block; the
appropriate transfer parameters
must be loaded with values.
Special cycle calls are also
possible with an additional
MCALL or CALL.

Programming principles
1.1 Fundamentals of programming
Turning Part 2: Programming (Siemens instructions)
20 Programming and Operating Manual, 05/2012, 6FC5398-5DP10-0BA0
Address Significance Value assignments Information Programming
CYCLE81 Drilling, centering N5 RTP=110 RFP=100
.... ; Assign with values
N10 CYCLE81(RTP,
RFP, ...); separate part
program block
CYCLE82 Drilling, counterboring N5 RTP=110 RFP=100
.... ;assign with values
N10 CYCLE82(RTP,
RFP, ...) ;separate block
CYCLE83 Deep-hole drilling N10 CYCLE83(110, 100,
...) ;or transfer values
directly
, separate block
CYCLE84 Rigid tapping N10 CYCLE84(...)
;separate block
CYCLE840 Tapping with compensating chuck N10 CYCLE840(...)
;separate block
CYCLE85 Reaming 1 N10 CYCLE85(...)
;separate block
CYCLE86 Boring N10 CYCLE86(...)
;separate block
CYCLE87 Drilling with stop 1 N10 CYCLE87(...);
separate part program
block
CYCLE88 Drilling with stop 2 N10 CYCLE88(...)
;separate block
CYCLE89 Reaming 2 N10 CYCLE89(...);
separate part program
block
CYCLE92 Cut-off N10 CYCLE92(...)
;separate block
CYCLE93 Recess N10 CYCLE93(...)
;separate block
CYCLE94 Undercut DIN76 (forms E and F), finishing N10 CYCLE94(...)
;separate block
CYCLE95 Stock removal with relief cutting N10 CYCLE95(...)
;separate block
CYCLE96 Thread undercut N10 CYCLE96(...);
separate part program
block
CYCLE98 Side-by-side thread mounting N10 CYCLE98(...);
separate part program
block
CYCLE99 Thread cutting N10 CYCLE99(...)
;separate block