Siemens SINUMERIK 840D Operating instructions

SINUMERIK
840D/840Di/810D/FM-NC
Cycles
Programming Guide
User Documentation
04.2000 Edition

SINUMERIK
840D/810D/
FM-NC
SINUMERIK
Overview of SINUMERIK 840D/840Di/810D/FM-NC Documentation (04.00)
Brochure Catalog
Ordering Info
NC 60.1 *)
Technical Info.
NC 60.2
Description of
Functions
Drive Functions *)
Description of
Functions
-- Basic Machine *)
-- Extended Functions
-- Special Functions
SINUMERIK
611D
840D/810D
SINUMERIK
840D/840Di/
810D/
FM-NC
840D/840Di/
810D/
FM-NC/611
Accessories
Catalog
Accessories NC-Z
SINUMERIK
SIROTEC
SIMODRIVE
840D/840Di/
810D
FM-NC
611D
Lists *)
Installation &
Start-up Guide *)
-- F M - N C
-- 810D
-- 840D/611D
-- MMC
SINUMERIK
840D
Description of
Functions
Digitizing
SINUMERIK
SINUMERIK
840D/810D/
FM-NC
Configuring Kit
MMC 100/101
-- Configuring
Syntax
-- Development Kit
SINUMERIK
840D/810D/
FM-NC
Screen Kit
MMC 100/101
SW Update and
Configuration
SINUMERIK
840D/840Di/
810D/
FM-NC
SINUMERIK
840D/840Di/
810D
Operator
Components
(HW) *)
840D/840Di/
810D/
FM-NC
Description of
Functions
SINUMERIK
Safety Integrated
SINUMERIK
SIMODRIVE
SINUMERIK
840D/810D/
FM-NC
611,
Motors
SIMODRIVE
DOCONCD*)
The SINUMERIK System
General Documentation
Electronic Documentation
Manufacturer / Service Documentation
Manufacturer / Service Documentation
SINUMERIK
840D/810D/
FM-NC
SINUMERIK
840D/810D
User Documentation
Diagnostics
Guide *)
Operator’s Guide
-- Unit
Operator Panel
-- HPU
-- HT 6
AutoTurn
-- Short Guide
-- Programming (1)
-- S e t u p ( 2 )
SINUMERIK
840D/840Di/
810D/
FM-NC
Program. Guide
-- Short Guide
-- Fundamentals *)
-- Advanced *)
-- Cycles
-- Measuring Cycles
Description of
Functions
-- ManualTurn
-- ShopMill
Description of
Functions
Synchronized
Actions
Wood, Glass,
Ceramics
840D/810D
SINUMERIK
Operator’s Guide
-- ManualTurn
-- Short Guide ManualTurn
-- ShopMill
-- Short Guide ShopMill
840D/810D
Manufacturer / Service Documentation
SINUMERIK
840D/810D
Descr. of Functions
-- Computer Link
-- Tool Data
Information
System
*) These documents are a minimum requirement for the control
Operator’s Guide
-- Short Guide
-- Operator’s
Guide *)
SINUMERIK
840D/810D/
FM-NC
Configuring
(HW) *)
-- F M - N C
-- 810D
-- 840D
SINUMERIK
SINUMERIK
840D/810D
SINUMERIK
840D/810D/
FM-NC
Description of
Functions
Operator Interface
OP 030
Description of
Functions
Tool Manage-
ment
SINUMERIK
SIMODRIVE SINUMERIK SIMODRIVE
SINUMERIK
SIMODRIVE
SINUMERIK
SIMODRIVE SINUMERIK
SIMODRIVE
840D
611D
840D
611D
Description of
Functions
Linear Motor
SINUMERIK
SIMODRIVE
SIROTEC
EMC
Guidelines
Description of
Functions
-- Hydraulics
Module
-- Analog Module
User Documentation
SINUMERIK
System Overview
840Di
Manufacturer / Service Documentation
SINUMERIK
Descr. of Functions
ISO Dialects for
SINUMERIK
840D/810D
SINUMERIK
Descr. of Functions
CAM Integration
DNC NT-2000
SINUMERIK
Manual
(HW + Installation
and Start-up)
840Di

SINUMERIK
840D/840Di/810D/FM-NC
04.00 Edition
Programming Guide
General 1
Drilling Cycles and
Drilling Patterns
2
Milling Cycles 3
Turning Cycles 4
Error Messages and
Error Handling
5
Appendix A
Cycles
Valid for
Control Software Version
SINUMERIK 840D 5
SINUMERIK 840Di 5
SINUMERIK 840DE (export version) 5
SINUMERIK 810D 3
SINUMERIK 810DE (export version) 3
SINUMERIK FM-NC 3

0Contents 04.00 0
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:
A .... New documentation.
B .... Unrevised edition with new Order No.
C .... Revised edition with new status.
If factual changes have been made on the page since the last edition, this is indicated by a
new edition coding in the header on that page.
Edition Order No. Remarks
02.95 6FC5298-2AB40-0BP0 A
04.95 6FC5298-2AB40-0BP1 C
03.96 6FC5298-3AB40-0BP0 C
08.97
12.97
6FC5298-4AB40-0BP0
6FC5298-4AB40-0BP1
C
C
12.98 6FC5298-5AB40-0BP0 C
08.99 6FC5298-5AB40-0BP1 C
04.00 6FC5298-5AB40-0BP2 C
This manual is included in the documentation available on CD ROM (DOCONCD)
Edition Order No. Remarks
04.00 6FC5 298-5CA00-0BG2 C
Trademarks
SIMATIC, SIMATIC HMI, SIMATIC NET, SIROTEC, SINUMERIKand SIMODRIVEare trademarks of
Siemens. Other names mentioned in this publication might be trademarks whose use by a third party for his
purposes could violate the rights of the holder.
Further information is available on the Internet under:
http://www.ad.siemens.de/sinumerik
This publication was produced with WinWord V 7.0
and Designer V 7.0.
The reproduction, transmission or use of this document or its contents is not
permitted without express written authority. Offenders will be liable for damages.
All rights, including rights created by patent grant or registration of a utility model
or design, are reserved.
© Siemens AG 1995, 1996, 1997, 1998, 1999, 2000. All Rights Reserved.
Other functions not described in this documentaion might be executable in the
control. This does not, however, represent an obligation to supply such functions
with a new control or when servicing.
We have checked that the contents of this document correspond to the hardware
and software described. Nonetheless, differences might exist and we, therefore,
cannot guarantee that they are completely identical. The information contained in
this document is, however, reviewed regularly and any necessary changes will be
included in the next edition. We welcome suggestions for improvement.
Subject to change without prior notice.
Order No. 6FC5298-5AB40-0BP2
Printed in the Federal Republic of Germany
Siemens-Aktiengesellschaft.

004.00 Contents 0
Siemens AG 2000 All rights reserved.
SINUMERIK 840D/840Di/810D/FM-NC Programming Guide Cycles (PGZ) - 04.00 Edition 0-5
Contents
General 1-15
1.1 General information ........................................................................................................ 1-16
1.2 Overview of cycles .......................................................................................................... 1-16
1.2.1 Drilling cycles, drill pattern cycles, milling cycles and turning cycles ........................ 1-17
1.2.2 Cycle auxiliary subroutines ....................................................................................... 1-18
1.3 Programming cycles ....................................................................................................... 1-19
1.3.1 Call and return conditions ......................................................................................... 1-19
1.3.2 Machine data ............................................................................................................ 1-20
1.3.3 Messages during execution of a cycle...................................................................... 1-21
1.3.4 Cycle call and parameter list..................................................................................... 1-22
1.3.5 Simulation of cycles .................................................................................................. 1-25
1.4 Cycle support in program editor (SW 4.3 and later) ....................................................... 1-26
1.4.1 Overview of important files ....................................................................................... 1-27
1.4.2 Configuring cycle selection ....................................................................................... 1-28
1.4.3 Configuring input screenforms for parameter assignment ....................................... 1-30
1.4.4 Configuring help displays.......................................................................................... 1-33
1.4.5 Configuring tools (MMC 100 only) ............................................................................ 1-34
1.4.6 Loading to the control ............................................................................................... 1-35
1.4.7 Independence of language ....................................................................................... 1-36
1.4.8 Operating the cycles support function....................................................................... 1-37
1.4.9 Integrating user cycles into the MMC 103 simulation function.................................. 1-38
1.5 Cycles support in the program editor (SW 5.1 and later)............................................... 1-39
1.5.1 Menus, cycle selection.............................................................................................. 1-39
1.5.2 New functions in input screenforms.......................................................................... 1-40
Drilling Cycles and Drilling Patterns 2-47
2.1 Drilling cycles ................................................................................................................. 2-48
2.1.1 Preconditions ............................................................................................................ 2-50
2.1.2 Drilling, centering –CYCLE81 .................................................................................. 2-52
2.1.3 Drilling, counterboring –CYCLE82 ........................................................................... 2-55
2.1.4 Deep-hole drilling –CYCLE83 .................................................................................. 2-57
2.1.5 Rigid tapping –CYCLE84 ......................................................................................... 2-65
2.1.6 Tapping with compensating chuck –CYCLE840...................................................... 2-69
2.1.7 Boring 1 –CYCLE85................................................................................................. 2-75
2.1.8 Boring 2 –CYCLE86................................................................................................. 2-78
2.1.9 Boring 3 –CYCLE87................................................................................................. 2-82
2.1.10 Boring 4 –CYCLE88................................................................................................. 2-85
2.1.11 Boring 5 –CYCLE89................................................................................................. 2-87
2.2 Modal call of drilling cycles............................................................................................. 2-89

0Contents 04.00 0
Siemens AG 2000 All rights reserved.
0-6 SINUMERIK 840D/840Di/810D/FM-NC Programming Guide Cycles (PGZ) - 04.00 Edition
2.3 Drill pattern cycles .......................................................................................................... 2-92
2.3.1 Preconditions ............................................................................................................ 2-92
2.3.2 Row of holes –HOLES1 ........................................................................................... 2-93
2.3.3 Hole circle –HOLES2 ............................................................................................... 2-97
2.3.4 Dot matrix –CYCLE801 (SW 5.3 and later) ........................................................... 2-100
Milling cycles 3-103
3.1 General information...................................................................................................... 3-104
3.2 Preconditions................................................................................................................ 3-105
3.3 Thread cutting - CYCLE90 ........................................................................................... 3-107
3.4 Elongated holes on a circle - LONGHOLE................................................................... 3-113
3.5 Slots on a circle - SLOT1 ............................................................................................. 3-119
3.6 Circumferential slot - SLOT2........................................................................................ 3-127
3.7 Milling rectangular pockets - POCKET1....................................................................... 3-132
3.8 Milling circular pockets - POCKET2............................................................................. 3-136
3.9 Milling rectangular pockets - POCKET3....................................................................... 3-140
3.10 Milling circular pockets - POCKET4 ............................................................................ 3-150
3.11 Face milling - CYCLE71............................................................................................... 3-156
3.12 Path milling - CYCLE72................................................................................................ 3-162
3.13 Milling rectangular spigots - CYCLE76 (SW 5.3 and later) .......................................... 3-172
3.14 Milling circular spigots - CYCLE77 (SW 5.3 and later)................................................. 3-177
3.15 Pocket milling with islands - CYCLE73, CYCLE74, CYCLE75 (SW 5.2 and later) ...... 3-181
3.15.1 Transfer pocket edge contour - CYCLE74.............................................................. 3-182
3.15.2 Transfer island contour - CYCLE75 ........................................................................ 3-184
3.15.3 Contour programming ............................................................................................. 3-185
3.15.4 Pocket milling with islands - CYCLE73 ................................................................... 3-188
Turning cycles 4-209
4.1 General information...................................................................................................... 4-210
4.2 Preconditions................................................................................................................ 4-211
4.3 Grooving cycle –CYCLE93.......................................................................................... 4-214
4.4 Undercut cycle –CYCLE94.......................................................................................... 4-223
4.5 Stock removal cycle –CYCLE95 ................................................................................. 4-227
4.6 Thread undercut –CYCLE96....................................................................................... 4-239
4.7 Thread cutting –CYCLE97 .......................................................................................... 4-243

004.00 Contents 0
Siemens AG 2000 All rights reserved.
SINUMERIK 840D/840Di/810D/FM-NC Programming Guide Cycles (PGZ) - 04.00 Edition 0-7
4.8 Thread chaining –CYCLE98 ....................................................................................... 4-251
4.9 Thread recutting (SW 5.3 and later) ............................................................................ 4-258
4.10 Extended stock removal cycle - CYCLE950 (SW 5.3 and later).................................. 4-260
Error Messages and Error Handling 5-281
5.1 General information ..................................................................................................... 5-282
5.2 Troubleshooting in the cycles....................................................................................... 5-282
5.3 Overview of cycle alarms ............................................................................................. 5-283
5.4 Messages in the cycles................................................................................................ 5-288
Appendix A-289
A Abbreviations ............................................................................................................... A-290
B Terms........................................................................................................................... A-299
C References................................................................................................................... A-309
D Index ......................................................................................................................................

0Preface 04.00
Structure of the manual 0
Siemens AG 2000 All rights reserved.
0-8 SINUMERIK 840D/840Di/810D/FM-NC Programming Guide Cycles (PGZ) - 04.00 Edition
Structure of the manual
The SINUMERIK documentation is organized in 3 parts:
•General Documentation
•User Documentation
•Manufacturer/Service Documentation
Target group
This documentation is intended for users of machine
tools. This publication provides detailed information
that the user requires for operating the SINUMERIK
FM-NC, 810D and 840D controls.
Standard scope
This programming guide describes the standard
functions. Differences and additions implemented by
the machine-tool manufacturer are documented by
the machine manufacturer.
More detailed information about other publications
concerning SINUMERIK FM-NC, 810D and 840D
and publications that apply to all SINUMERIK
controls (e.g. Universal Interface, Measuring
Cycles...) can be obtained from your local Siemens
branch office.
Other functions not described in this documentation
might be executable in the control. This does not,
however, represent an obligation to supply such
functions with a new control or when servicing.
Applicability
This Programming Guide applies to: SINUMERIK
FM-NC, 810D, 840D or 840Di control systems with
MMC 100 and MMC 102/103.
Details of software versions in the Programming Guide
refer to the 840D system, but apply correspondingly to
the 810D, e.g. SW 5 on a SINUMERIK 840D
corresponds to SW 3 on a SINUMERIK 810D.

004.00 Preface
Structure of the manual 0
Siemens AG 2000 All rights reserved.
SINUMERIK 840D/840Di/810D/FM-NC Programming Guide Cycles (PGZ) - 04.00 Edition 0-9
Structure of descriptions
All cycles and program functions were laid out
according to the same structure, as far as possible
and practicable. The various levels of information
have been structured so that you can find the
information you are looking for quickly.
1. The function at a glance
If you need to look up a cycle that is rarely
used or the meaning of a parameter, you will
see at a glance how the function is programmed
together with an explanation of the cycles and
parameters.
This information always appears at the beginning of
the page.
Note:
In order to keep the documentation succinct we have
not provided all the methods or representation of the
individual cycles and parameters that are possible in
the programming language. Cycles have been
programmed in the form in which they most
frequently arise on the shop floor.
2
Drilling cycles and drilling patterns 03.96
2.1 Drillin
g
c
y
cles 2
Siemens AG 1997 All rights reserved.
2-36
SINUMERIK 840D/810D/FM-NC Programming Guide, Cycles (PGZ) - 08.97 Edition.
2.1.2 Drilling, centering – CYCLE81
Programming
CYCLE81 (RTP, RFP, SDIS, DP)
RTP real Retraction plane (absolute)
RFP real Reference plane (absolute)
SDIS real Safety clearance (enter without sign)
DP real Final drilling depth (absolute)
DPR real Final drilling depth relative to reference plane (enter without sign)
Function
The tool drills at the programmed spindle speed and
feedrate to the programmed final drilling depth.
X
Z
Operating sequence
Position reached before the beginning of the
cycle:
The drilling position is the position in the two axes of
the selected plane.
The cycle implements the following motion
sequence:
• Approach of the reference plane brought forward
by the safety clearance with G0
• Travel to the final drilling depth at the feedrate
programmed in the calling program (G1)
• Retraction to retraction plane with G0

0Preface 04.00
Structure of the manual 0
Siemens AG 2000 All rights reserved.
0-10 SINUMERIK 840D/840Di/810D/FM-NC Programming Guide Cycles (PGZ) - 04.00 Edition
2. Detailed explanations
In the theoretical sections, you are provided with a
detailed description of the following:
What is the cycle used for?
What does the cycle do?
What is the sequence of operations?
What do the parameters do?
What else do you have to look out for?
The theoretical sections provide learning material for
the NC beginner. You should work through the
manual at least once to get an idea of the scope of
the functions and capability of your SINUMERIK
control.
2
03.96 Drilling cycles and drilling patterns
2.1 Drillin
g
c
y
cles 2
Siemens AG 1997 All rights reserved.
SINUMERIK 840D/810D/FM-NC Programming Guide, Cycles (PGZ) - 08.97 Edition.
2-37
Explanation of parameters
RFP and RTP
Generally, the reference plane (RFP) and the
retraction plane (RTP) have different values. In the
cycle it is assumed that the retraction plane lies in
front of the reference plane. The distance between
the retraction plane and the final drilling depth is
therefore greater than the distance between the
reference plane and the final drilling depth.
SDIS
The safety clearance (SDIS) refers to the reference
plane. which is brought forward by the safety
clearance. The direction in which the safety
clearance is active is automatically determined by
the cycle.
DP and DPR
The drilling depth can be defined either absolute
(DP) or relative (DPR) to the reference plane.
If it is entered as an absolute value, the value is
traversed directly in the cycle.
G1
G0
RTP
RFP+SDIS
RFP
DP=RFP-DPR
X
Z
Additional notes
If a value is entered both for the DP and the DPR,
the final drilling depth is derived from the DPR. If the
DPR deviates from the absolute depth programmed
via the DP, the message "Depth: Corresponds to
value for relative depth" is output in the dialog line.
3. From theory to practice
The programming example shows you how to
include the cycles in an operating sequence.
An application example of almost all the cycles is
provided after the theoretical section.
2
Drilling cycles and drilling patterns 03.96
2.1 Drillin
g
c
y
cles 2
Siemens AG 1997 All rights reserved.
2-38
SINUMERIK 840D/810D/FM-NC Programming Guide, Cycles (PGZ) - 08.97 Edition.
If the values for the reference plane and the
retraction plane are identical, a relative depth must
not be programmed. The error message
61101 "Reference plane incorrectly defined" is
output and the cycle is not executed. This error
message is also output if the retraction plane lies
behind the reference plane, i.e. the distance to the
final drilling depth is smaller.
Programming example
Drilling_centering
You can use this program to make 3 holes using the
drilling cycle CYCLE81, whereby this cycle is called
with different parameter settings. The drilling axis is
always the Z axis.
X
Y
40
B
90
30
0
120
35 100 108
A
A - B
Z
Y
N10 G0 G90 F200 S300 M3 Specification of the technology values
N20 D3 T3 Z110 Traverse to retraction plane
N30 X40 Y120 Traverse to first drilling position
N40 CYCLE81 (110, 100, 2, 35) Cycle call with absolute final drilling
depth, safety clearance and incomplete
parameter list
N50 Y30 Traverse to next drilling position
N60 CYCLE81 (110, 102, , 35) Cycle call without safety clearance
N70 G0 G90 F180 S300 M03 Specification of the technology values
N80 X90 Traverse to next position
N90 CYCLE81 (110, 100, 2, , 65) Cycle call with relative final drilling depth
and safety clearance
N100 M30 End of program
08.97

004.00 Preface
Structure of the manual 0
Siemens AG 2000 All rights reserved.
SINUMERIK 840D/840Di/810D/FM-NC Programming Guide Cycles (PGZ) - 04.00 Edition 0-11
Explanation of symbols
Sequence of operations
Explanation
Function
Parameters
Sample program
Programming
Additional notes
Cross-reference to other documentation or sections
Danger notes and sources of error
Additional notes or background information

0Preface 04.00
Pro
p
er use 0
Siemens AG 2000 All rights reserved.
0-12 SINUMERIK 840D/840Di/810D/FM-NC Programming Guide Cycles (PGZ) - 04.00 Edition
Warning notes
The following warning notes with graded degrees of
importance are used in this documentation.
Danger
This symbol appears whenever death, serious
personal injury or substantial material damage will
occur if the appropriate precautions are not taken.
Caution
This symbol appears whenever minor personal injury
can occur if the appropriate precautions are not
taken.
Warning
This symbol appears whenever death, serious
personal injury or substantial material damage can
occur if the appropriate precautions are not taken.

004.00 Preface
Pro
p
er use 0
Siemens AG 2000 All rights reserved.
SINUMERIK 840D/840Di/810D/FM-NC Programming Guide Cycles (PGZ) - 04.00 Edition 0-13
Principle
Your SIEMENS 810D, 840D and FM-NC have been
designed and constructed to the latest standards of
technology and recognized safety rules, standards
and regulations.
Additional equipment
The applications of SIEMENS controls can be
expanded by adding special additional devices,
equipment and expansion units supplied by
SIEMENS.
Personnel
Only authorized and reliable personnel who have
been trained in the use of the equipment may be
allowed to handle the control. Nobody without the
necessary training must be allowed to operate the
control, even temporarily.
The corresponding responsibilities of personnel
who set up, operate and maintain the equipment
must be clearly defined and adherence to these
responsibilities monitored.
Behavior
Before the control is started up, the personnel who
are to work on the control must be thoroughly
acquainted with the Operator’s Guides. The
operating company is also responsible for
constantly monitoring the overall technical state of
the control (noticeable faults and damage, altered
service performance).

0Preface 04.00
Pro
p
er use 0
Siemens AG 2000 All rights reserved.
0-14 SINUMERIK 840D/840Di/810D/FM-NC Programming Guide Cycles (PGZ) - 04.00 Edition
Servicing
Repairs must be carried out by personnel who are
specially trained and qualified in the relevant
technical subject according to the information
supplied in the service and maintenance guide. All
relevant safety regulations must be followed.
Note
The following is deemed to be improper usage and
exempts the manufacturer from any liability:
Any application which does not comply with the rules
for proper usage described above.
If the control is not in technically perfect condition
or is operated without due regard for safety
regulations and accident prevention instructions
given in the Instruction Manual.
If faults that might affect the safety of the equipment
are not rectified before the control is started up.
Any modification, bypassing or disabling of items
of equipment on the control that are required to
ensure fault-free operation, unlimited use and active
and passive safety.
Improper usage gives rise to unforeseen dangers
to:
•life and limb of personnel
•the control, machine and other assets of the
owner and the user may result.

112.97 General 1
Siemens AG 2000 All rights reserved.
SINUMERIK 840D/840Di/810D/FM-NC Programming Guide, Cycles (PGZ) - 04.00 Edition 1-15
General
1.1 General information ........................................................................................................ 1-16
1.2 Overview of cycles .......................................................................................................... 1-16
1.2.1 Drilling cycles, drill pattern cycles, milling cycles and turning cycles ....................... 1-17
1.2.2 Cycle auxiliary subroutines ...................................................................................... 1-18
1.3 Programming cycles ....................................................................................................... 1-19
1.3.1 Call and return conditions ........................................................................................ 1-19
1.3.2 Machine data ........................................................................................................... 1-20
1.3.3 Messages during execution of a cycle..................................................................... 1-21
1.3.4 Cycle call and parameter list.................................................................................... 1-22
1.3.5 Simulation of cycles ................................................................................................. 1-25
1.4 Cycle support in program editor (SW 4.3 and later) ....................................................... 1-26
1.4.1 Overview of important files ...................................................................................... 1-27
1.4.2 Configuring cycle selection ...................................................................................... 1-28
1.4.3 Configuring input screenforms for parameter assignment ...................................... 1-30
1.4.4 Configuring help displays......................................................................................... 1-33
1.4.5 Configuring tools (MMC 100 only) ........................................................................... 1-34
1.4.6 Loading to the control .............................................................................................. 1-35
1.4.7 Independence of language ...................................................................................... 1-36
1.4.8 Operating the cycles support function ..................................................................... 1-37
1.4.9 Integrating user cycles into the MMC 103 simulation function................................. 1-38
1.5 Cycle support in the program editor (SW 5.1 and later) ................................................. 1-39
1.5.1 Menus, cycle selection............................................................................................. 1-39
1.5.2 New functions in input screenforms......................................................................... 1-40

1General 12.97
1.1 General information 1
Siemens AG 2000 All rights reserved.
1-16 SINUMERIK 840D/840Di/810D/FM-NC Programming Guide, Cycles (PGZ) - 04.00 Edition
1.1 General information
The first section provides you with an overview of the
available cycles. The following sections describe the
general conditions that apply to all cycles regarding
•programming the cycles and
•operator guidance for calling the cycles.
1.2 Overview of cycles
Cycles are generally applicable technology
subroutines with which you can implement specific
machining operations such as tapping a thread or
milling a pocket. These cycles are adapted to
individual tasks by parameter assignment.
The system provides you with various standard
cycles for the technologies
•Drilling
•Milling
•Turning.

1
12.97 General
1.2
Overview of cycles
1
Siemens AG 2000 All rights reserved.
SINUMERIK 840D/840Di/810D/FM-NC Programming Guide, Cycles (PGZ) - 04.00 Edition 1-17
1.2.1 Drilling cycles, drill pattern cycles, milling cycles and turning cycles
You can perform the following cycles with the
SINUMERIK FM-NC, 810D and 840D control:
Drilling cycles
CYCLE81 Drilling, centering
CYCLE82 Drilling, counterboring
CYCLE83 Deep hole drilling
CYCLE84 Rigid tapping
CYCLE840 Tapping with floating tapholder
CYCLE85 Boring 1
CYCLE86 Boring 2
CYCLE87 Boring 3
CYCLE88 Boring 4
CYCLE89 Boring 5
Drill pattern cycles
HOLES1 Machining a row of holes
HOLES2 Machining a circle of holes
New in SW 5.3 and higher:
CYCLE801 Dot matrix
Milling cycles
LONGHOLE Milling pattern of elongated holes on a circle
SLOT1 Milling pattern of slots arranged on a circle
SLOT2 Milling pattern of circumferential slots
POCKET1 Rectangular pocket milling (with face cutter)
POCKET2 Circular pocket milling (with face cutter)
CYCLE90 Thread milling
New in SW 4 and higher:
POCKET3 Rectangular pocket milling (with any milling tool)
POCKET4 Circular pocket milling (with any milling tool)
CYCLE71 Face milling
CYCLE72 Contour milling
04.00

1
General 12.97
1.2 Overview of c
y
cles
1
Siemens AG 2000 All rights reserved.
1-18 SINUMERIK 840D/840Di/810D/FM-NC Programming Guide, Cycles (PGZ) - 04.00 Edition
New in SW 5.2 and higher:
CYCLE73 Pocket milling with islands
CYCLE74 Transfer of pocket edge contour
CYCLE75 Transfer of island contour
New in SW 5.3 and higher:
CYCLE76 Mill a rectangular spigot
CYCLE77 Mill a circular spigot
Turning cycles
CYCLE93 Groove
CYCLE94 Undercut (form E and F according to DIN)
CYCLE95 Stock removal with relief cut
CYCLE96 Thread undercut (forms A, B, C and D according to
DIN)
CYCLE97 Thread cutting
CYCLE98 Chaining of threads
New in SW 5.1 and higher:
CYCLE950 Extended stock removal
1.2.2 Cycle auxiliary subroutines
The following auxiliary routines are part of the cycles
package
•PITCH and
•MESSAGE.
These must always be loaded in the control.
04.00

1
12.97 General
1.3
Programming cycles
1
Siemens AG 2000 All rights reserved.
SINUMERIK 840D/840Di/810D/FM-NC Programming Guide, Cycles (PGZ) - 04.00 Edition 1-19
1.3 Programming cycles
A standard cycle is defined as a subroutine with a
name and a parameter list. The conditions described
in "SINUMERIK Programming Guide Part 1:
Fundamentals" apply when calling a cycle.
The cycles are supplied on diskette or, for the
MMC102, with the corresponding software release.
They are loaded into the part program memory of
the control via the V.24 interface (see Operator’s
Guide).
1.3.1 Call and return conditions
The G functions active before the cycle is called and
the programmable frame remain active beyond the
cycle.
You define the machining plane (G17, G18, G19)
before calling the cycle. A cycle operates in the
current plane with
•Abscissa (1st geometrical axis)
•Ordinate (2nd geometrical axis)
•Applicate (3rd geometrical axis of the plane in
space).
In drilling cycles, the hole is machined in the axis
that corresponds to the applicate of the current
plane. The depth infeed is performed in this axis with
milling applications.
Ordinate
Abscissa
Y
X
Z
Applicate
G19
G18
G17
Plane and axis assignments
Command Plane Perpendicular infeed axis
G17 X/Y Z
G18 Z/X Y
G19 Y/Z X

1
General 12.97
1.3 Pro
g
rammin
g
c
y
cles
1
Siemens AG 2000 All rights reserved.
1-20 SINUMERIK 840D/840Di/810D/FM-NC Programming Guide, Cycles (PGZ) - 04.00 Edition
1.3.2 Machine data
The following machine data are used for the cycles.
The minimum values for these machine data are
given in the table below.
Relevant machine data
MD No. MD name Minimum value
18118 MM_NUM_GUD_MODULES 7
18130 MM_NUM_GUD_NAMES_CHAN 10
18150 MM_GUD_VALUES_MEM 10
18170 MM_NUM_MAX_FUNC_NAMES 40
18180 MM_NUM_MAX_FUNC_PARAM 400
28020 MM_NUM_LUD_NAMES_TOTAL 200
28040 MM_NUM_LUD_VALUES_MEM 25
The machine data files are delivered with these
defaults by the machine manufacturer.
It is important to remember that a power ON must be
performed if these machine data are changed.
Axis-specific machine data MD 30200: NUM_ENCS
must also be noted with respect to cycle CYCLE840
(tapping with compensating chuck).
05.98