Siemens SINUMERIK 802D sl Owner's manual

Validity
Software Version
SINUMERIK 840D/DE powerline 7.4
SINUMERIK 840Di/DiE powerline 3.3
SINUMERIK 810D/DE powerline 7.4
SINUMERIK 840D sl/DE sl 1.4
SINUMERIK 840Di sl/DiE sl 1.4
SINUMERIK 802D sl 1.4
04.2007 Edition
Programming Manual ISO Turning
SINUMERIK 802D sl840D/ 840D sl
840Di/840Di sl/810D
Programming GuideProgramming GuideProgramming GuideProgramming GuideProgramming GuideProgramming GuideProgramming GuideProgramming GuideProgramming GuideProgramming GuideProgramming GuideProgramming GuideProgramming GuideProgramming GuideProgramming GuideProgramming GuideProgramming Guide
Programming Basics 1
Commands Calling
Axis Movements 2
Movement Control
Commands 3
Enhanced Level
Commands 4
Appendix
Abbreviations A
Terms B
G Code Table C
MDs and SDs D
Data Fields, Lists E
Alarms F
Index

SINUMERIK®documentation
Printing history
Brief details of this edition and previous editions are listed below.
The status of each edition is shown by the code in the “Remarks” column.
Status code in the “Remarks” column:
ANew documentation......
BUnrevised reprint with new Order No......
CRevised edition with new status......
Edition Order No. Remarks
02.01 6FC5 298--6AC10--0BP0 A
12.01 6FC5 298--6AC10--0BP1 C
11.02 6FC5 298--6AC10--0BP2 C
04.05 6FC5 298--7AC10--0BP0 C
04.07 6FC5398--5BP10--0BA0 C
Trademarks
All product designations could be trademarks or product names of Siemens AG or other
companies which, if used by third parties, could infringe the rights of theier owners.
Exclusion of liability
We have checked the contents of the documentation for consistency with the hardware and software
described. Since deviations cannot be precluded entirely, we cannot guarantee complete conformance.
The information in this document is regularly checked and necessary corrections are included in reprints.
Suggestions for improvement are also welcome.
Siemens--Aktiengesellschaft
©Siemens AG 005. All rights reserved.
Printed in the Federal Re
p
ublic of German
y
3ls

iii
©SIEMENS AG 2007 All rights reserved
SINUMERIK 802D sl/840D sl840D/840Di sl/840Di/810D ISO Turning -- 04.07 Edition
Preface
Structure of the documentation
The SINUMERIK documentation is structured in three levels:
SGeneral documentation
SUser documentation
SManufacturer/service documentation.
An overview of publications that is updated monthly is provided in a number of lan-
guages in the Internet at:
http://www.siemens.com/motioncontrol
Follow menu items > ”Support” > ”Technical Documentation” > ”Overview of Docu-
ments”.
DOConWEB, the Internet edition of DOConCD, is available at:
http://www.automation.siemens.com/doconweb
Information on the training courses offered as well as FAQs (frequently asked
questions) are provided on the Internet at:
http://www.siemens.com/motioncontrol, ”Support” menu item.
Target audience
This documentation is intended for:
SProject engineers
STechnologists (from machine manufacturers)
SSystem startup (Systems/Machines
SProgrammers
Standard scope
This documenation only describes the functionality if the standard version. Exten-
sions or changes made by the machine tool manufacturer are documented by the
machine tool manufacturer.
It may be possible to runfunctions that are not described in this document in your
controller. This does not, however, represent an obligation to supply such functions
with a new control or when servicing.
Further, for the sake of simplicity, this documentation does not contain all detailed
information about all types of the product and cannot cover every conceivable case
of installation, operation or maintenance.

Preface 04.07
iv ©SIEMENS AG 2007 All rights reserved
SINUMERIK 802D sl/840D sl840D/840Di sl/840Di/810D ISO Turning -- 04.07 Edition
Technical Support
If you have any questions, please get in touch with our Hotline:
Europe / Africa Asia / Australia America
Phone [phone] [phone] [phone]
Fax [phone] [phone] [phone]
Internet http:// www.siemens.com/automation/support--request
E--Mail mailto:[e-mail]
Note
Should you require technical support, please call one of the country--specific
phone numbers provided on the Internet:
http://www.siemens.com/automation/services&support
Questions regarding the manual
If you have any queries (suggestions, corrections) in relation to this documentation,
please send a fax or e--mail to the following address:
Fax [phone]
E--Mail mailto:[e-mail]
Fax form: see reply form at the end of the manual.
SINUMERIK Internet address
http://www.siemens.com/sinumerik
Origin
In contrast to the Siemens mode programming of YASKAWA SIEMENS 840DI,
ISO dialect programming is mainly based on SINUMERIK 6T--B and SINUMERIK
6M--B, a CNC control which had already been phased out. However, OEM and en-
duser requirements on SINUMERIK 6T--B programming compatibility lead to the
development of the ISO dialect function.

Preface
04.07
v
©SIEMENS AG 2007 All rights reserved
SINUMERIK 802D sl/840D sl840D/840Di sl/840Di/810D ISO Turning -- 04.07 Edition
Safety Instructions
This manual contains information which you should carefully observe to ensure
your own personal safety and the prevention of material damage. These notices
referring to your personal safety are highlighted by a safety alert symbol. The noti-
ces referringto property damage alone have no safety alert symbol. The warnings
appear in decreasing order of risk as given below.
!Danger
indicates that death or severe personal injury will result if proper precautions are
not taken.
!Warning
indicates that death or severe personal injury can result if proper precautions are
not taken.
!Caution
with a warning triangle indicates that minor personal injury can result if proper pre-
cautions are not taken.
Caution
without warning triangle indicates that material damage can result if proper precau-
tions are not taken.
Notice
indicates that an undesirable event or state may arise if the relevant notes are not
observed.
If several hazards of different degree occur, the hazard with the highest degree
must always be given priority. If a warning note with a warning triangle warns of
personal injury, the same warning note can also contain a warning of material da-
mage.

Preface 04.07
vi ©SIEMENS AG 2007 All rights reserved
SINUMERIK 802D sl/840D sl840D/840Di sl/840Di/810D ISO Turning -- 04.07 Edition
Qualified personnel
The associated device/system may only be set up and operated using this docu-
mentation. Commissioning and operation of a device/system may only be perfor-
med by qualified personnel. Qualified persons are defined as persons who are
authorized to commission, to ground, and to tag circuits, equipment, and systems
in accordance with established safety practices and standards.
Prescribed Usage
Please note the following:
!Warning
The equipment may only be used for single purpose applications explicitly descri-
bed in the catalog and in the technical description and it may only be used along
with third--party devices and components recommended by Siemens. To ensure
trouble--free and safe operation of the product, it must be transported, stored and
installed as intended and maintained and operated with care.
Further notes
Note
This icon is displayed in the present documentation whenever additional facts are
being specified.

Table of Contents
04.07
vii
©SIEMENS AG 2007 All rights reserved
SINUMERIK 802D sl/840D sl840D/840Di sl/840Di/810D ISO Turning -- 04.07 Edition
Table of Contents
1 Programming Basics 1-11...................................................
1.1 Introductory explanations 1-11.........................................
1.1.1 Siemens mode 1-11..................................................
1.1.2 ISO Dialect mode 1-11...............................................
1.1.3 Switchover 1-12.....................................................
1.1.4 G code display 1-12..................................................
1.1.5 Maximum number of axes / axis designation 1-12........................
1.1.6 Selection of G code system A, B, or C 1-13.............................
1.1.7 Decimal point programming 1-13.......................................
1.1.8 Comments 1-15.....................................................
1.1.9 Block skip 1-16......................................................
1.2 Basics of feed function 1-17...........................................
1.2.1 Rapid traverse 1-17..................................................
1.2.2 Cutting feed (F command) 1-17........................................
1.2.3 Switching between feed per minute mode and feed per revolution mode
(G94/G95) 1-21......................................................
2 Commands Calling Axis Movements 2-23.....................................
2.1 Interpolation commands 2-23..........................................
2.1.1 Positioning (G00) 2-23................................................
2.1.2 Linear interpolation (G01) 2-25........................................
2.1.3 Circular interpolation (G02, G03) 2-27..................................
2.1.4 Cylindrical interpolation (G07.1) 2-33...................................
2.1.5 Polar coordinate interpolation (G12.1, G13.1) 2-35.......................
2.2 Using the thread cutting function 2-38..................................
2.2.1 Thread cutting and continuous thread cutting (G33) 2-38..................
2.2.2 Continuous thread cutting 2-41........................................
2.2.3 Multiple-thread cutting (G33) 2-43......................................
2.2.4 Variable lead thread cutting (G34) 2-46.................................
2.3 Reference point return 2-47...........................................
2.3.1 Automatic return to reference point (G28) 2-47...........................
2.3.2 Reference point return check (G27) 2-49................................
2.3.3 Second to fourth reference point return (G30) 2-50.......................
2.3.4 Rapid lift with G10.6 2-51.............................................
2.4 Tool retract (G10.6) 2-53..............................................
3 Movement Control Commands 3-55..........................................
3.1 The coordinate system 3-55...........................................
3.1.1 Machine coordinate system (G53) 3-56.................................
3.1.2 Workpiece coordinate system (G92) 3-57...............................
3.1.3 Resetting the work (G92.1) 3-57.......................................
3.1.4 How to select a workpiece coordinate system 3-58.......................
3.1.5 Instantaneous mapping of the ISO functions onto the Siemens frames
(until powerline 7.04.2, solution line 1.4) 3-59............................
3.1.6 Uncoupling the frames between the Siemens and the ISO modes
(with powerline 7.04.02 or solution line 1.4 and higher) 3-61...............

Table of Contents 04.07
viii ©SIEMENS AG 2007 All rights reserved
SINUMERIK 802D sl/840D sl840D/840Di sl/840Di/810D ISO Turning -- 04.07 Edition
3.2 Determining the coordinate value input modes 3-66......................
3.2.1 Absolute/incremental designation 3-66..................................
3.2.2 Diametric and radial commands for X-axis 3-69..........................
3.2.3 Inch/metric input designation (G20, G21) 3-70...........................
3.2.4 G60: Oriented positioning 3-71........................................
3.3 Time-controlling commands 3-72.......................................
3.3.1 Dwell (G04) 3-72....................................................
3.4 Tool offset functions 3-73.............................................
3.4.1 Tool offset data memory 3-73..........................................
3.4.2 Tool position offset 3-73...............................................
3.4.3 Tool nose radius compensation function (G40, G41/G42) 3-73.............
3.5 Spindle function (S function) 3-80......................................
3.5.1 Spindle command (S5-digit command) 3-80.............................
3.5.2 Constant surface speed control (G96, G97) 3-81.........................
3.6 Tool function (T function) 3-84.........................................
3.7 Miscellaneous function (M function) 3-84................................
3.7.1 M codes relating to stop operation (M00, M01, M02, M30) 3-84............
3.7.2 Internally processed M codes 3-85.....................................
3.7.3 Macro call via M function 3-85.........................................
3.7.4 General purpose M codes 3-86........................................
4 Enhanced Level Commands 4-89.............................................
4.1 Program support functions (1) 4-89.....................................
4.1.1 Canned cycles 4-89..................................................
4.1.2 Multiple repetitive cycles 4-101.........................................
4.1.3 Hole-machining canned cycles (G80 to G89) 4-118........................
4.2 Program support functions (2) 4-129.....................................
4.2.1 Changing of tool offset value
Programmable data input (G10) 4-129...................................
4.2.2 Subprogram call up function (M98, M99) 4-130...........................
4.3 Eight-digit program number 4-134.......................................
4.4 Automating support functions 4-135.....................................
4.4.1 Skip function (G31) 4-135..............................................
4.4.2 Multistage skip (G31, P1--P2) 4-138.....................................
4.5 Macroprograms 4-139.................................................
4.5.1 Differences from subprograms 4-139....................................
4.5.2 Macroprogram call (G65, G66, G67) 4-139...............................
4.6 Advanced functions 4-147..............................................
4.6.1 High--speed cycle cutting (G05) 4-147...................................
4.6.2 Polygonal turning 4-148................................................
4.6.3 Compressor in ISO dialect mode 4-150..................................
4.6.4 Switchover modes for DryRun and skip levels 4-151.......................
4.6.5 Interrupt programm with M96 / M97 (ASUP) 4-152........................

Table of Contents
04.07
ix
©SIEMENS AG 2007 All rights reserved
SINUMERIK 802D sl/840D sl840D/840Di sl/840Di/810D ISO Turning -- 04.07 Edition
A Abbreviations A-155..........................................................
B Terms B-165..................................................................
C G Code Table C-195...........................................................
C.1 G code table C-195....................................................
D Machine and Setting Data D-199...............................................
D.1 Machine/Setting Data D-199............................................
D.2 Channel-specific machine data D-212....................................
D.3 Axis-specific setting data D-219.........................................
D.4 Channel-specific setting data D-220.....................................
E Data Fields, Lists E-223.......................................................
E.1 Machine data E-223...................................................
E.2 Setting data E-226....................................................
E.3 Variables E-226.......................................................
F Alarms F-229.................................................................
G Commands I-231.............................................................
Index I-233..................................................................

Table of Contents 04.07
x©SIEMENS AG 2007 All rights reserved
SINUMERIK 802D sl/840D sl840D/840Di sl/840Di/810D ISO Turning -- 04.07 Edition
Notes

Programming Basics
1.1 Introductory explanations
04.07
1-11
©SIEMENS AG 2007 All rights reserved
SINUMERIK 802D sl/840D sl840D/840Di sl/840Di/810D ISO Turning -- 04.07 Edition
Programming Basics
1.1 Introductory explanations
1.1.1 Siemens mode
The following conditions apply when Siemens mode is active:
SSiemens G commands are interpreted on the control by default. This applies to
all channels.
SIt is not possible to extend the Siemens programming system with ISO Dialect
functions because some of the G functions have different meanings.
SDownloadable MD files can be used to switch the control to ISO Dialect mode.
In this case, the system boots the ISO Dialect mode by default.
1.1.2 ISO Dialect mode
The following conditions apply when ISO Dialect mode is active:
SOnly ISO Dialect G codes can be programmed, not Siemens G codes.
SIt is not possible to use a mixture of ISO Dialect code and Siemens code in the
same NC block.
SIt is not possible to switch between ISO Dialect--M and ISO Dialect--T via
G command.
SSiemens subprogram calls can be programmed.
SIf further Siemens functions are to be used, it is necessary to switch to Siemens
mode first.
1

Programming Basics
1.1 Introductory explanations
04.07
1-12 ©SIEMENS AG 2007 All rights reserved
SINUMERIK 802D sl/840D sl840D/840Di sl/840Di/810D ISO Turning -- 04.07 Edition
1.1.3 Switchover
The following two G commands are 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 in a separate NC program block.
The active tool, the tool offsets and the zero offsets are not changed by this action.
1.1.4 G code display
The G code display must always be implemented in the same language type
(Siemens/ISO Dialect) as the current block display. If the block display is suppres-
sed with DISPLOF, the current G codes continue to be displayed in the language
type of the active block.
Example
The Siemens standard cycles are called up using the G functions of the ISO Dia-
lect mode. DISPLOF is programmed at the start of the cycle, with the result that
the ISO Dialect G commands remain active for the display.
PROC CYCLE328 SAVE DISPLOF
N10 ...
...
N99 RET
Procedure
External main program calls Siemens shell cycle. Siemens mode is selected impli-
citly on the shell cycle call.
DISPLOF freezes the block display at the call block; the G code display remains in
external mode. This display is refreshed while the Siemens cycle is running.
The SAVE attribute resets the G codes modified in the shell cycle to their original
state when the shell cycle was called on the return jump to the main program.
1.1.5 Maximum number of axes / axis designation
In ISO Dialect--T the maximum number of axis is 8. Axis designation for the first
two axes is fixed to X and Z. Further axes can be designated Y, A, B, C, U, V, W.

Programming Basics
1.1 Introductory explanations
04.07
1-13
©SIEMENS AG 2007 All rights reserved
SINUMERIK 802D sl/840D sl840D/840Di sl/840Di/810D ISO Turning -- 04.07 Edition
1.1.6 Selection of G code system A, B, or C
ISO Dialect T distinguishes between G code system A, B, and C. G code system B
is default setting. The G code system in use is selected by MD $MN_MM_EX--
TERN_GCODE_SYSTEM 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 G code system A is active, G91 is not available. In this case, incremental axes
movement for axis X,Y, and Z is programmed by address U, V, and W. U, V, and W
are not available as axis designation in this case resulting in a maximum axes
number of 6.
Address H is used for programming incremental movement of the C axis in G code
system A.
Notice
SIf not otherwise noted, the manual in hand describes G code system B.
SFor the differences between G code system A, B, and C refer to the G code list
in the appendix.
1.1.7 Decimal point programming
There are two notations for the interpretation of programming values without a
decimal point in ISO Dialect mode:
Spocket calculator type notation
Values without decimal points are interpreted as mm, inch or degrees.
Sstandard notation
Values without decimal points are multiplied by a conversion factor.
The setting is defined by MD 10884, see Chapter 4 “Startup”.
There are two different conversion factors, IS-B and IS-C. This evaluation refers to
addresses X Y Z U V W A B C I J K Q R and F.
Example of linear axis in mm:
X 100.5 corresponds to value with decimal point: 100.5mm
X 1000 pocket calculator type notation: 1000mm
standard notation: IS-B: 1000* 0.001= 1mm
IS-C: 1000* 0.0001 = 0.1mm

Programming Basics
1.1 Introductory explanations
04.07
1-14 ©SIEMENS AG 2007 All rights reserved
SINUMERIK 802D sl/840D sl840D/840Di sl/840Di/810D ISO Turning -- 04.07 Edition
ISO-Dialekt Milling
Table 1-1 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 deg 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 min.) mm
inch
0.01
0.0001
0.01
0.0001
F thread pitch 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
Qmm
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 s0.001 0.001
A contour angle deg 0.001 0.0001
G74, G84 thread drilling cycles
$MC_EXTERN_FUNCTION_MASK
Bit8 = 0 F feedrate like G94, G95
Bit8 = 1 F thread pitch
ISO dialekt Turning
Table 1-2 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 deg 0.001 0.0001
F feed G94 (mm/inch pro min.) mm
inch
1
0.01
1
0.01
F feed G95 (mm/inch pro Umdr.)
$MC_EXTERN_FUNCTION_MASK
Bit8 = 0 mm
inch
0.01
0.0001
0.01
0.0001

Programming Basics
1.1 Introductory explanations
04.07
1-15
©SIEMENS AG 2007 All rights reserved
SINUMERIK 802D sl/840D sl840D/840Di sl/840Di/810D ISO Turning -- 04.07 Edition
Table 1-2 Different conversion factors for IS-B and IS-C
Address IS-CIS-BUnit
Bit8 = 1 mm
inch
0.0001
0.00000
1
0.0001
0.00000
1
F thread pitch mm
inch
0.0001
0.00000
1
0.0001
0.00000
1
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
I, J, K interpolation parameters mm
inch
0.001
0.0001
0.0001
0.00001
G04 X or U 0.001 0.001
A contour angle 0.001 0.0001
G76, G78 thread drilling cycles
$MC_EXTERN_FUNCTION_MASK
Bit8 = 0 F feedrate like G94, G95
Bit8 = 1 F thread pitch
G84, G88 thread drilling cycles
$MC_EXTERN_FUNCTION_MASK
Bit9 = 0 G95 F mm
inch
0.01
0.0001
0.01
0.0001
Bit8 = 1 G95 F mm
inch
0.0001
0.00000
1
0.0001
0.00000
1
1.1.8 Comments
In ISO dialect mode, round brackets are interpreted as comment characters.
In Siemens mode, “;” is interpreted as a comment. To simplify matters, “;” is also
interpreted as a comment in ISO dialect model.
If the comment start character “(” is used again within a comment, the comment
will not be terminated until all open brackets have been closed again.
Example:
N5 (comment) X100 Y100
N10 (comment(comment)) X100 Y100
N15 (comment(comment) X100) Y100
In blocks N5 and N10 X100 Y100 is executed, in block N15 only Y100, as the first
bracket is closed only after X100. Everything up to this position is interpreted as a
comment.

Programming Basics
1.1 Introductory explanations
04.07
1-16 ©SIEMENS AG 2007 All rights reserved
SINUMERIK 802D sl/840D sl840D/840Di sl/840Di/810D ISO Turning -- 04.07 Edition
1.1.9 Block skip
The skip character “/” can be anywhere within the block, even in the middle. If the
programmed skip level is active at the moment of compiling, the block will not be
compiled from this position to the end of the block. An active skip level therefore
has the same effect as an end of block.
Example:
N5 G00 X100. /3 YY100 ----> Alarm 12080,
N5 G00 X100. /3 YY100 ----> No alarm when skip level 3 is active
Skip characters within a comment are not interpreted as skip characters.
Example:
N5 G00 X100. ( /3 part1 ) Y100 ;even when skip level 3 is active, the
;Y axis will be traversed
The skip level can be /1 to /9. Skip values <1 >9 give rise to alarm 14060
The function is mapped onto the existing Siemens skip levels. In contrast to ISO
Dialect Original, / and /1 are separate skip levels and therefore have to be
activated separately.
Notice
S“1” can be omitted for “/1”.
SThe optional block skip function is processed when a part program is read to
the buffer register from either the tape or memory. If the switch is set ON after
the block containing the optional block skip code is read, the block is not skip-
ped.
SThe optional block skip function is disregarded for program reading (input) and
punch out (output) operation.

Programming Basics
1.2 Basics of feed function
04.07
1-17
©SIEMENS AG 2007 All rights reserved
SINUMERIK 802D sl/840D sl840D/840Di sl/840Di/810D ISO Turning -- 04.07 Edition
1.2 Basics of feed function
This section describes the feed function that specifies feedrate (distance per
minute, distance per revolution) of a cutting tool.
1.2.1 Rapid traverse
Rapid traverse is used for positioning (G00) and manual rapid traverse (RAPID)
operation. In the rapid traverse mode, each axis moves at the rapid traverse rate
set for the individual axes; the rapid traverse rate is determined by the machine
tool builder and set for the individual axes by using parameters. Since the axes
move independently of each other, the axes reach the target point at different time.
Therefore, the resultant tool paths are not a straight line generally.
1.2.2 Cutting feed (F command)
The feedrate at which a cutting tool should be moved in the linear interpolation
(G01) mode or circular interpolation (G02, G03) mode is designated using address
characters F. The axis feed mode to be used is selected by designating the feed
function G code (G94 or G95) as indicated in Table 1-3. Select the required feed
mode by designating the feed function G code before specifying an F code.
Table 1-3 Cutting feed mode G codes
G code Function Group
G94 Designation of feed per minute (mm/min) mode 05
G95 Designation of feed per revolution (mm/rev) mode 05
See 1.2.3 “Switching between feed per minute mode and feed per revolution
mode” for details of these G codes. The F code is modal and once designated it
remains valid until another F code is designated. If feed mode designation G codes
are switched between G94 and G95, however, it is necessary to designate the
F code again. If no new F code is designated, alarm 10860 “No feedrate program-
med” occurs.
Feed per revolution mode (G95)
A feedrate of a cutting tool per revolution of the spindle (mm/rev, inch/rev) can be
designated by a numeral specified following address character F.
Note: The upper limit of feedrates could be restricted by the servo system and the mechani-
cal system. For the actual programmable feedrate range, refer to the manuals pub-
lished by the machine tool builder.

Programming Basics
1.2 Basics of feed function
04.07
1-18 ©SIEMENS AG 2007 All rights reserved
SINUMERIK 802D sl/840D sl840D/840Di sl/840Di/810D ISO Turning -- 04.07 Edition
An F command specified in the simultaneous 2-axis linear interpolation mode or in
the circular interpolation mode represents the feedrate in the tangential direction.
Example of programming (linear interpolation mode)
300 mm/min
400 mm/min
+X
+Z
Tangential velocity
500 mm/min
G95 S1000 (r/min);
G91 G01 X60. Z40. F0.5;
Fig. 1-1 F command in simultaneous 2-axis control linear interpolation (feed per revolution)
Example of programming (circular interpolation mode)
Center
200 mm/min
Fx
Fz
+Z
+X
G95 S1000 (r/min);
G91 G03 X ... Z ... I ... F0.2;
Fig. 1-2 F command in the simultaneous 2-axis control circular interpolation (feed per
revolution)
Notice
SAn F0 command causes an input error.
SA feedrate in the X-axis direction is determined by the radial value.
A feedrate of a cutting tool per minute (mm/min, inch/min) can be designated by
a numeral specified following address character F.

Programming Basics
1.2 Basics of feed function
04.07
1-19
©SIEMENS AG 2007 All rights reserved
SINUMERIK 802D sl/840D sl840D/840Di sl/840Di/810D ISO Turning -- 04.07 Edition
Notice
The upper limit of feedrates could be restricted by the servo system and the mechanical
system. For the actual programmable feedrate range, refer to the manuals published by the
machine tool builder.
Simultaneous 2-axis control
An F command specified in the simultaneous 2-axis linear interpolation mode or in
the circular interpolation mode represents the feedrate in the tangential direction.
Example of programming (linear interpolation mode)
300 mm/min
400 mm/min
+X
+Z
Tangential velocity
500 mm/min
G94;
G91 G01 X60. Z40. F500.;
Fig. 1-3 F command in simultaneous 2-axis control linear interpolation (feed per minute)
Notice
SAn F0 command causes an input error.
SA feedrate in the X-axis direction is determined by the radial value.

Programming Basics
1.2 Basics of feed function
04.07
1-20 ©SIEMENS AG 2007 All rights reserved
SINUMERIK 802D sl/840D sl840D/840Di sl/840Di/810D ISO Turning -- 04.07 Edition
Example of programming (circular interpolation mode) Center
200 mm/min
Fx
Fz
+Z
+X
G94;
G91 G03 X ... Z .. I ... F200.;
Fig. 1-4 F command in the simultaneous 2-axis control circular interpolation (feed per
minute)
Notice
Do not specify a negative value for an F command.
Rotary axis and linear axis
An F command specified in the interpolation mode between a rotary axis and a
linear axis represents the feedrate in the tangential direction.
Example of programming
10 mm
60 deg
+C
+Z
Tangential velocity
100 mm/min
G94 G91;
G01 Z10. C60. F100.;
Fig. 1-5 F command in interpolation between rotary axis and linear axis (feed per minute)