Siemens SINUMERIK 808D User manual

© Siemens AG 2017. All rights reserved
6FC5398-4DP10-0BA6, 09/2017 1
SINUMERIK
SINUMERIK 808D, SINUMERIK 808D ADVANCED
Programming and Operating Manual (Milling)
User Manual
Legal information
Warning notice system
This manual contains notices you have to observe in order to ensure your personal safety, as well as to prevent damage to property. The
notices referring to your personal safety are highlighted in the manual by a safety alert symbol, notices referring only to property damage
have no safety alert symbol. These notices shown below are graded according to the degree of danger.
DANGER
indicates that death or severe personal injury willresult if proper precautions are not taken.
W A R NING
indicates that death or severe personal injury may result if proper precautions are not taken.
C AUTION
indicates that minor personal injury can result if proper precautions are not taken.
N O TICE
indicates that property damage can result if proper precautions are not taken.
If more than one degree of danger is present, the warning notice representing the highest degree of danger will be used. A notice warning of
injury to persons with a safety alert symbol may also include a warning relating to property damage.
Qualified Personnel
The product/systemdescribed 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:
W A R NING
Siemens products may only be used for the applications described in the catalog and in the relevant technical documentation. If products
and components from other manufacturers are used, these must be recommended or approved by Siemens. Proper transport, storage,
installation, assembly, commissioning, operation and maintenance are required to ensure that the products operate safely and without any
problems. The permissible ambient conditions must be complied with. The information in the relevant documentation must be observed.

Programming and Operating Manual (Milling)
26FC5398-4DP10-0BA6, 09/2017
Preface
Applicable products
This manual is valid for the following control systems:
Control system Software version
SINUMERIK 808D ADVANCED M (Milling) V4.8.1.2: PPU16x.3/PPU15x.3 with spindle/feed servo system
SINUMERIK 808D (Milling) V4.8.1.1: PPU141.3 with feed servo system
Documentation components and target audience
End-user documentation Target audience
Programming and Operating Manual (Turning) Programmers and operators ofturning machines
Programming and Operating Manual (Milling) Programmers and operators ofmilling machines
Programming and Operating Manual (ISO Turning/Milling) Programmers and operators ofturning/milling machines
Programming and Operating Manual (Manual Machine
Plus (MM+), Turning)
Programmers and operators ofturning machines
Diagnostics Manual Mechanical and electrical designers,commissioning engi-
neers, machine operators,and service and maintenance per-
sonnel
Manufacturer/service documentation Target audience
Commissioning Manual Installation personnel,commissioning engineers,and service
and maintenance personnel
Function Manual Mechanical and electrical designers,technical professionals
Parameter Manual Mechanical and electrical designers,technical professionals
Service Manual Mechanical and electrical designers,technical professionals,
commissioning engineers,and service and maintenance per-
sonnel
Readme file
Third-party software - Licensing terms and copyrightinformation
My Documentation Manager (MDM)
Under the following link you will find information to individually compile your documentation based on the Siemenscontent:
www.siemens.com/mdm
Standard scope
This manual only describes the functionality of the standard version. Extensions or changes made by the machine tool
manufacturer are documented bythe machine tool manufacturer.
Technical support
Country Hotline 1) Further service contact information:
•Worldwide Web site:
https://support.industry.siemens.com/cs/ww/en/
•Chinese Web site:
http://www.siemens.com.cn/808D
Germany [phone]
China [phone]
1) You can find more hotline information atthe worldwide Web site given above.

Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017 3
EC Declaration of Conformity
The EC Declaration ofConformity for the EMC Directive can be found on the Internet at
http://www.siemens.com/automation/service&support.
Here, enter the number "
67385845
" as the search term or contact your local Siemens office.

Programming and Operating Manual (Milling)
46FC5398-4DP10-0BA6, 09/2017
Table of contents
Preface............................................................................................................................................... 2
1 Fundamental safety instructions .............................................................................................................. 8
1.1 General safety instructions.....................................................................................................................................8
1.2 Warranty and liability for application examples...................................................................................................8
1.3 Industrial security.....................................................................................................................................................9
2 Introduction......................................................................................................................................... 9
2.1 Panel Processing Units (PPUs).............................................................................................................................9
2.1.1 PPU versions............................................................................................................................................................9
2.1.2 PPU control elements.......................................................................................................................................... 10
2.1.3 Screen layout......................................................................................................................................................... 12
2.2 Machine Control Panels (MCPs)........................................................................................................................ 13
2.2.1 MCP versions........................................................................................................................................................ 13
2.2.2 MCP control elements.......................................................................................................................................... 13
2.3 Coordinate systems.............................................................................................................................................. 16
2.4 Protection levels.................................................................................................................................................... 18
3 Common notices for machining operations............................................................................................... 20
4 Switching on and referencing................................................................................................................ 20
5 Setting the user interface language ........................................................................................................ 21
6 Setting up tools.................................................................................................................................. 21
6.1 Creating a tool....................................................................................................................................................... 21
6.2 Creating/changing a cutting edge...................................................................................................................... 22
6.3 Activating the tool and the spindle..................................................................................................................... 23
6.4 Assigning the handwheel..................................................................................................................................... 24
6.4.1 Assigning the handwheel through the MCP..................................................................................................... 24
6.4.2 Assigning the handwheel through the PPU...................................................................................................... 25
6.5 Measuring the tool manually............................................................................................................................... 27
6.6 Verifying the tool offset result............................................................................................................................. 28
7 Creating part programs........................................................................................................................ 29
7.1 Creating a part program....................................................................................................................................... 29
7.2 Editing the part program...................................................................................................................................... 31
7.2.1 Using a standard program structure.................................................................................................................. 31
7.2.2 Editing a part program ......................................................................................................................................... 31
7.2.3 Understanding frequently used programming instructions............................................................................ 37
7.2.3.1 Inch or metric dimensions (G70/G71)............................................................................................................... 37
7.2.3.2 Definition of work offset (G54 to G59, G500, G90/G91) ................................................................................ 37
7.2.3.3 Rapid traverse (G00)............................................................................................................................................ 38
7.2.3.4 Tool and traverse (T, D, M6, F, G94/G95, S, M3/M4, G01) .......................................................................... 39
7.2.3.5 Tool radius compensation (G40, G41/G42) ..................................................................................................... 39
7.2.3.6 Milling circles and arcs (G02/G03)..................................................................................................................... 40
7.2.3.7 Fixed point approach (G74/G75)........................................................................................................................ 41
7.2.3.8 Spindle control....................................................................................................................................................... 42
7.2.3.9 Setting dwell time in the program (G04)........................................................................................................... 42
8 Program simulation............................................................................................................................. 42
8.1 Simulation prior to machining of the workpiece............................................................................................... 43
8.2 Simultaneous recording prior to machining of the workpiece........................................................................ 45
9 Machining the workpiece...................................................................................................................... 46

Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017 5
9.1 Executing a part program.....................................................................................................................................46
9.2 Executing specified blocks...................................................................................................................................47
9.3 Correcting a part program....................................................................................................................................48
9.4 Simultaneous recording during machining of the workpiece..........................................................................48
9.5 Entering the tool wear offsets..............................................................................................................................49
10 Other common operations ....................................................................................................................53
10.1 Program control functions....................................................................................................................................53
10.1.1 Program test...........................................................................................................................................................53
10.1.2 Dry run feedrate.....................................................................................................................................................53
10.1.3 Conditional stop.....................................................................................................................................................53
10.1.4 Skip block...............................................................................................................................................................53
10.1.5 Single block mode.................................................................................................................................................53
10.1.6 Rapid traverse override........................................................................................................................................54
10.1.7 Auxiliary function lock...........................................................................................................................................54
10.2 Calibrating the tool probe.....................................................................................................................................54
10.3 Measuring the tool with a probe (auto)..............................................................................................................56
10.4 Setting up the workpiece......................................................................................................................................57
10.4.1 Measuring the workpiece.....................................................................................................................................57
10.4.2 Entering/modifying workpiece offsets ................................................................................................................59
10.5 Entering/modifying the setting data....................................................................................................................60
10.6 Setting R parameters............................................................................................................................................63
10.7 Setting user data...................................................................................................................................................64
10.8 Setting the date and time.....................................................................................................................................64
10.9 Configuring the operating area after startup .....................................................................................................65
10.10 Executing/transferring a part program from external.......................................................................................65
10.10.1 Executing/transferring through the USB interface............................................................................................65
10.10.1.1 Executing from external (through USB interface)............................................................................................66
10.10.1.2 Transferring from external (through USB interface)........................................................................................67
10.10.2 Executing/transferring through the Ethernet connection.................................................................................67
10.10.2.1 Configuring the network drive..............................................................................................................................67
10.10.2.2 Executing from external (through Ethernet connection)..................................................................................70
10.10.2.3 Transferring from external (through Ethernet connection)..............................................................................70
10.10.3 Configuring the firewall.........................................................................................................................................71
10.11 Extending/deactivating the CNC lock function..................................................................................................72
10.12 Data backup...........................................................................................................................................................74
10.12.1 Internal data backup.............................................................................................................................................74
10.12.2 External data backup............................................................................................................................................75
10.12.2.1 External data backup in a data archive..............................................................................................................75
10.12.2.2 External data backup of separate files...............................................................................................................76
10.13 Pocket calculator...................................................................................................................................................77
11 Programming principles........................................................................................................................78
11.1 Fundamentals of programming...........................................................................................................................78
11.1.1 Program names.....................................................................................................................................................78
11.1.2 Program structure..................................................................................................................................................79
11.2 Programming instructions....................................................................................................................................79
11.2.1 Programming dimensions....................................................................................................................................79
11.2.2 Plane selection: G17 to G19................................................................................................................................80
11.2.3 Absolute/incremental dimensioning: G90, G91, AC, IC ..................................................................................81
11.2.4 Dimensions in metric units and inches: G71, G70, G710, G700...................................................................82
11.2.5 Polar coordinates, pole definition: G110, G111, G112....................................................................................82
11.2.6 Programmable work offset: TRANS, ATRANS.................................................................................................84
11.2.7 Programmable rotation: ROT, AROT.................................................................................................................85
11.2.8 Programmable scale factor: SCALE, ASCALE ................................................................................................86
11.2.9 Programmable mirroring: MIRROR, AMIRROR...............................................................................................87
11.2.10 Workpiece coordinate system - settable work offset: G54 to G59, G500, G53, G153 ..............................88

Programming and Operating Manual (Milling)
66FC5398-4DP10-0BA6, 09/2017
11.2.11 NC block compression (COMPON, COMPCURV, COMPCAD)................................................................... 89
11.3 Linear interpolation............................................................................................................................................... 91
11.3.1 Linear interpolation with rapid traverse: G0...................................................................................................... 91
11.3.2 Feedrate F............................................................................................................................................................. 92
11.3.3 Linear interpolation with feedrate: G1 ............................................................................................................... 92
11.4 Circular interpolation............................................................................................................................................ 93
11.4.1 Circular interpolation: G2, G3 ............................................................................................................................. 93
11.4.2 Circular interpolation via intermediate point: CIP............................................................................................ 98
11.4.3 Circle with tangential transition: CT................................................................................................................... 99
11.4.4 Helix interpolation: G2/G3, TURN...................................................................................................................... 99
11.4.5 Feedrate override for circles: CFTCP, CFC ...................................................................................................100
11.5 Thread cutting.....................................................................................................................................................101
11.5.1 Thread cutting with constant lead: G33 ..........................................................................................................101
11.5.2 Tapping with compensating chuck: G63.........................................................................................................102
11.5.3 Thread interpolation: G331, G332...................................................................................................................103
11.6 Fixed point approach..........................................................................................................................................104
11.6.1 Fixed point approach: G75................................................................................................................................104
11.6.2 Reference point approach: G74.......................................................................................................................105
11.7 Acceleration control and exact stop/continuous path...................................................................................105
11.7.1 Acceleration pattern: BRISK, SOFT ................................................................................................................105
11.7.2 Exact stop/continuous-path control mode: G9, G60, G64 ...........................................................................106
11.7.3 Dwell time: G4.....................................................................................................................................................108
11.8 Spindle movements............................................................................................................................................109
11.8.1 Gear stages.........................................................................................................................................................109
11.8.2 Spindle speed S, directions of rotation............................................................................................................109
11.8.3 Spindle positioning: SPOS................................................................................................................................110
11.9 Contour programming support..........................................................................................................................110
11.9.1 Contour definition programming.......................................................................................................................110
11.9.2 Rounding, chamfer.............................................................................................................................................112
11.10 Tool and tool offset.............................................................................................................................................115
11.10.1 General Information............................................................................................................................................115
11.10.2 Tool T....................................................................................................................................................................116
11.10.3 Tool compensation number D...........................................................................................................................116
11.10.4 Selecting the tool radius compensation: G41, G42.......................................................................................119
11.10.5 Corner behavior: G450, G451..........................................................................................................................121
11.10.6 Tool radius compensation OFF: G40 ..............................................................................................................122
11.10.7 Special cases of the tool radius compensation..............................................................................................123
11.10.8 Example of tool radius compensation.............................................................................................................124
11.11 Miscellaneous function M..................................................................................................................................125
11.12 H function.............................................................................................................................................................125
11.13 Arithmetic parameters, LUD and PLC variables............................................................................................126
11.13.1 Arithmetic parameter R......................................................................................................................................126
11.13.2 Local User Data (LUD).......................................................................................................................................127
11.13.3 Reading and writing PLC variables..................................................................................................................128
11.14 Program jumps....................................................................................................................................................129
11.14.1 Unconditional program jumps...........................................................................................................................129
11.14.2 Conditional program jumps...............................................................................................................................129
11.14.3 Program example for jumps..............................................................................................................................131
11.14.4 Jump destination for program jumps...............................................................................................................132
11.15 Subroutine technique.........................................................................................................................................132
11.15.1 General information............................................................................................................................................132
11.15.2 Calling machining cycles...................................................................................................................................134
11.15.3 Modal subroutine call.........................................................................................................................................134
11.15.4 Executing internal and external subroutines (CALL, EXTCALL)................................................................135
11.16 Timers and workpiece counters.......................................................................................................................136
11.16.1 Runtime tim er......................................................................................................................................................136
11.16.2 Workpiece counter..............................................................................................................................................138
11.17 Smooth approach and retraction......................................................................................................................139

Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017 7
11.18 Cylinder surface transformation (TRACYL)................................................................................................... 144
11.19 Coupled motion (TRAILON, TRAILOF) .......................................................................................................... 150
12 Cycles............................................................................................................................................ 152
12.1 Overview of cycles............................................................................................................................................. 152
12.2 Programming cycles.......................................................................................................................................... 153
12.3 Graphical cycle programming in the program editor..................................................................................... 154
12.4 Drilling cycles...................................................................................................................................................... 155
12.4.1 General information............................................................................................................................................ 155
12.4.2 Requirem ents...................................................................................................................................................... 156
12.4.3 Drilling, centering - CYCLE81 .......................................................................................................................... 157
12.4.4 Drilling, counterboring - CYCLE82.................................................................................................................. 159
12.4.5 Deep-hole drilling - CYCLE83.......................................................................................................................... 161
12.4.6 Rigid tapping - CYCLE84.................................................................................................................................. 166
12.4.7 Tapping with compensating chuck - CYCLE840........................................................................................... 170
12.4.8 Reaming 1 - CYCLE85...................................................................................................................................... 175
12.4.9 Boring - CYCLE86.............................................................................................................................................. 176
12.5 Drilling pattern cycles......................................................................................................................................... 179
12.5.1 Requirem ents...................................................................................................................................................... 179
12.5.2 Row of holes - HOLES1.................................................................................................................................... 179
12.5.3 Circle of holes - HOLES2.................................................................................................................................. 182
12.5.4 Arbitrary positions - CYCLE802....................................................................................................................... 185
12.6 Milling cycles....................................................................................................................................................... 186
12.6.1 Requirem ents...................................................................................................................................................... 186
12.6.2 Face milling - CYCLE71.................................................................................................................................... 187
12.6.3 Contour milling - CYCLE72............................................................................................................................... 192
12.6.4 Milling a rectangular spigot - CYCLE76.......................................................................................................... 200
12.6.5 Milling a circular spigot - CYCLE77................................................................................................................. 204
12.6.6 Long holes located on a circle - LONGHOLE................................................................................................ 207
12.6.7 Slots on a circle - SLOT1 .................................................................................................................................. 211
12.6.8 Circumferential slot - SLOT2 ............................................................................................................................ 216
12.6.9 Milling a rectangular pocket - POCKET3........................................................................................................ 221
12.6.10 Milling a circular pocket - POCKET4............................................................................................................... 226
12.6.11 Thread milling - CYCLE90................................................................................................................................ 230
12.6.12 High speed settings - CYCLE832.................................................................................................................... 234
12.7Error messages and error handling................................................................................................................. 234
12.7.1 General Information........................................................................................................................................... 234
12.7.2 Error handling in the cycles.............................................................................................................................. 234
12.7.3 Overview of cycle alarms.................................................................................................................................. 235
12.7.4 Messages in the cycles..................................................................................................................................... 235
13 Machining typical milling parts ............................................................................................................. 235
13.1 Operations before programming...................................................................................................................... 235
13.2 Programming (Example 1)................................................................................................................................ 236
13.3 Programming (Example 2)................................................................................................................................ 245
13.4 Programming (Example 3)................................................................................................................................ 252
13.5 Programming (Example 4)................................................................................................................................ 267
13.6 Program simulation and execution.................................................................................................................. 278
A Appendix......................................................................................................................................... 279
A.1 Operating area overview................................................................................................................................... 279
A.1.1 Machining operating area.................................................................................................................................. 279
A.1.2 Program editing operating area....................................................................................................................... 279
A.1.3 Offset operating area......................................................................................................................................... 280
A.1.4 Program management operating area............................................................................................................ 281
A.1.5 System data operating area.............................................................................................................................. 284
A.1.6 Alarm operating area......................................................................................................................................... 286
A.2 Operating mode overview................................................................................................................................. 287
A.2.1 "JOG" m ode ........................................................................................................................................................ 287

Programming and Operating Manual (Milling)
86FC5398-4DP10-0BA6, 09/2017
A.2.1.1 Running the spindle manually..........................................................................................................................288
A.2.1.2 Executing M functions........................................................................................................................................289
A.2.1.3 Setting the relative coordinate system (REL).................................................................................................290
A.2.1.4 Face milling..........................................................................................................................................................291
A.2.1.5 Setting the JOG data..........................................................................................................................................293
A.2.2 "AUTO" mode......................................................................................................................................................294
A.2.3 "MDA" mode........................................................................................................................................................295
A.3 Activating the contour handwheel via the NC program ................................................................................296
A.4 The help system..................................................................................................................................................298
A.5 Operation wizard.................................................................................................................................................300
A.6 Editing Chinese characters...............................................................................................................................301
A.7 Calculating contour elements ...........................................................................................................................302
A.8 Free contour programming................................................................................................................................306
A.8.1 Defining a start point..........................................................................................................................................307
A.8.2 Programming contour element.........................................................................................................................308
A.8.3 Parameters for contour elem ents.....................................................................................................................311
A.8.4 Specifying contour elements in polar coordinates.........................................................................................314
A.8.5 Cycle support.......................................................................................................................................................316
A.8.6 Programming example formilling application................................................................................................316
A.9 Word structure and address..............................................................................................................................324
A.10 Character set.......................................................................................................................................................325
A.11 Block format.........................................................................................................................................................325
A.12 List of instructions...............................................................................................................................................327
1
Fundamental safety instructions
1.1
General safety instructions
WARNING
Danger to life if the safety instructions and residual risks are not observed
If the safety instructions and residual risks in the associated hardware
documentation are notobserved,accidents involving
severe injuriesor death can occur.
•Observe the safety instructions given in the hardware documentation.
•Considerthe residual risks for the risk evaluation.
WARNING
Malfunctions of the machine as a result of incorrect or changed parameter settings
As a resul
t of incorrect or changed parameterization,machines can malfunction,which in turn can lead to injuriesor death.
•Protect the parameterization (parameter assignments) againstunauthorized access.
•
Handle possible malfunctions bytaking suitable measures,e.g.emergencystop or emergencyoff.
1.2
Warranty and liability for application examples
The application examples are notbinding and do not claim to be complete regarding configuration,equipmentor any
eventuality which may arise.The application examples do not representspecific customer solutions, but are only intended to
provide supportfor typical tasks. You are responsible forthe properoperation of the described products.These application
examples do not relieve you of your responsibility for safe handling when using,installing,operating and maintaining the
equipment.

Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017 9
1.3
Industrial security
Note
Industrial security
Siemens provides products and solutions with industrial security functions that supportthe secure operation of plants,
systems, machines and networks.
In order to protect plants, systems, machinesand networks againstcyberthreats, it is necessaryto implement – and
continuously maintain – a holistic, state-of-the-art industrial security concept.Siemens products and solutions only rep
resent
one componentofsuch a concept.
The customer is responsible for preventing unauthorized access to its plants, systems, machinesand networks.Systems,
machinesand components should only be connected to the enterprise networkor the internetif and
to the extent necessary
and with appropriate security measures (e.g.use of firewalls and network segmentation) in place.
Additionally,Siemens’ guidance on appropriate security measuresshould be taken into account. For more information about
industrial security, please visit:
Industrial security (http://www.siemens.com/industrialsecurity).
Siemens’ productsand solutionsundergo continuous developmentto make them more secure. Siemens strongly
recommends to apply productupdates as soon as available and to always use the latest product versions.Use of product
versions that are no longer supported,and failure to apply latest updates may increase customer’s exposure to cyber
threats.
To stay informed about productupdates,subscribe to the Siemens Industrial Security RSS Feed at:
Industrial security (http://www.siemens.com/industrialsecurity).
WARNING
Unsafe operating states resulting from software manipulation
Software manipulations (e.g.viruses,trojans, malware or worms) can cause unsafe operating states in your system that
may lead to death, serious injury, and property damage.
•Keep the software up to date.
•Incorporate the automation and drive componentsinto a holistic,state-of-the-art industrial security conceptfor the
installation or machine.
•Make sure that you include all installed productsinto the holisticindustrial security concept.
•Protect files stored on exchangeable storage media from malicious software bywith suitable protection measures,e.g.
virus scanners.
2
Introduction
Note
Chapter"Machining typical milling parts (Page 235)"later in this manual provides you with typical machining examples
including workpiece drawings,typical programs,and step-by-step operating instructions.It helps you to quickly understand
CNC programming and operation through practical examples.
2.1
Panel Processing Units (PPUs)
2.1.1
PPUversions
PPU version
Technology variant
Operator panel variant
Applicable control system
PPU161.3
Turning variant
Horizontal panel, with English keys
SINUMERIK 808D ADVANCED T (Turning)
Horizontal panel, with Chinese keys
Milling variant
Horizontal panel, with English keys
SINUMERIK 808D ADVANCED M (Milling)
Horizontal panel, with Chinese keys
PPU160.3 Turning variant
Vertical panel,with English keys
SINUMERIK 808D ADVANCED T (Turning)
Vertical panel,with Chinese keys
Milling variant
Vertical panel,with English keys
SINUMERIK 808D ADVANCED M (Milling)
Vertical panel,with Chinese keys

Programming and Operating Manual (Milling)
10 6FC5398-4DP10-0BA6, 09/2017
PPU version
Technology variant
Operator panel variant
Applicable control system
PPU151.3 Turning variant Horizontal panel, with English keys SINUMERIK 808D ADVANCED T (Turning)
Horizontal panel, with Chinese keys
Milling variant
Horizontal panel, with English keys
SINUMERIK 808D ADVANCED M (Milling)
Horizontal panel, with Chinese keys
PPU150.3 Turning variant Vertical panel,with English keys SINUMERIK 808D ADVANCED T (Turning)
Vertical panel,with Chinese keys
Milling variant Vertical panel,with English keys SINUMERIK 808D ADVANCED M (Milling)
Vertical panel,with Chinese keys
PPU141.3 Turning variant Horizontal panel, with English keys SINUMERIK 808D (Turning)
Horizontal panel, with Chinese keys
Milling variant Horizontal panel, with English keys SINUMERIK 808D (Milling)
Horizontal panel, with Chinese keys
2.1.2
PPU control elements
①
Status indicators
⑧
Alarm cancellation key
Cancelsalarms and messages thatare marked with the
symbol on this key
②
Protective cover for USB interface
⑨
Wizard key
Guides you through performing basic commissio
ning
and operation tasks
③
U SB interface
⑩
Help key
Calls help information
④
Horizontal and vertical keys
Call the corresponding vertical/horizontal softkeys on
the screen
⑪
Cursor keys
⑤
Return key
Returns to the next higher-level menu
⑫
Modifier keys for use in key combinations
⑥
Menu extension key
Calls the extended menu items
⑬
Edit control keys
⑦
Alphabetic and numeric keys
⑭
Operating area keys

Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017 11
Additional information about keys
<CTRL + P>: Creates a screenshotof the actual user interface
<CTRL + S>: Saves start-up archives and action logs to a USB stick
<CTRL + D>: Displays pre-defined slideson the screen
<ALT + D>: Saves action logs to a USB stick
Calls the calculator function when you position the cursor on the desired inputfield
<CTRL + cursor key>: Changes the screen backlightbrightness by an increment of10% (bright-
ness range:10% to 100%)
Note that after you release the key combination, the HMI saves your brightnesssetting and the
brightness bar disappears after a few seconds.
Enters the upper character shown on the alphabetic/numeric keys concerned
+
Opens the system data operating area
In the program editor,pressing this key movesthe cursor to the beginning ofthe selected pro-
gram block.
•Toggles between entries in the input field
•Enters the "Set-up menu" dialog box at NC startup
Enables user-defined extension applications,forexample,generation ofuser dialog boxes with
the EasyXLanguage function.For more information aboutthis function,see the SINUMERIK
808D/SINUMERIK 808D ADVANCED Function Manual.
Status indicators
Indicator
Status and meaning
"POK"
•
Solid green:The powersupply for the control system is switched on.
"RDY"
•
Solid green:The control system is ready and the PLC is in run mode.
•Solid red: The control system is in stop mode.
•Solid orange:The PLC is in stop mode.
•
Flashing orange:The PLC is in power-up mode.
"TEMP" •Off: The temperature ofthe control system is within the specified scope.
•
Solid orange:The temperature of the control system is beyond the scope.

Programming and Operating Manual (Milling)
12 6FC5398-4DP10-0BA6, 09/2017
2.1.3
Screen layout
Alarms and messages in the status area
Displays active alarms with alarm text
The alarm number is displayed in white letter-
ing on a red background.The associated
alarm text is shown in red lettering. An arrow
indicates that several alarms are active. The
number to the right of the arrow indicatesthe
total number of active alarms.When more
than one alarm is active, the display scrolls
through the alarms in sequence.An acknowl-
edgementsymbol indicates the alarm cancel
criterion.
Displays messages from NC programs
Messages from NC programs do not have
numbersand appear in green lettering.

Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017 13
2.2
Machine Control Panels (MCPs)
2.2.1
MCP versions
MCP version
Applicable control system
•Horizontal MCP, with English keys and override switches
•
Horizontal MCP, with Chinese keys and override switches
•Vertical MCP, with English keys and a reserved slot for
the handwheel
•Vertical MCP, with Chinese keys and a reserved slot for
the handwheel
•Vertical MCP, with English keys and an override switch
for the spindle
•Vertical MCP, with Chinese keys and an override switch
for the spindle
All MCP variants are applicable to anyof the following
control systems:
•SINUMERIK 808D ADVANCED T (Turning)
•SINUMERIK 808D ADVANCED M (Milling)
•SINUMERIK 808D (Turning)
•SINUMERIK 808D (Milling)
2.2.2
MCP control elements
Horizontal MCP
Vertical MCP
•
Variant with an override switch for the spindle
•
Variant with a reserved slot for the handwheel
①
Reserved hole for emergency stop button
⑧
Feedrate override switch
②
Tool number display
Displays the number ofthe currently active tool
⑨
Spindle control keys

Programming and Operating Manual (Milling)
14 6FC5398-4DP10-0BA6, 09/2017
③
Operating mode selection area
⑩
Keys for program start, stop, and reset
④
Program control keys
⑪
Pre-defined labeling strips for keys of the MCP
⑤
User-defined keys
⑫
Reserved slot for the handwheel
⑥
Axis traversing keys
⑬
Spindle override control keys
⑦
Spindle override switch
Functions of user-defined keys
Switcheson/off the machine tool working lamp (always active independentofthe machine operating
mode)
Indicator on: The working lamp on the machine tool is switched on.
Indicator off: The working lamp on the machine tool is switched off.
Switches on/off of the coolantsupply (always active independent ofthe machine operating mode)
Indicator on: The coolantsupply is switched on.
Indicator off: The coolantsupply is switched off.
Controls the locking/unlocking ofthe safety door
Indicator on: The safety door is unlocked.
Indicator off: The safety door is locked.
Note:
If you want to unlockthe safety door, make sure all axesand the spindle have stopped running.
Controls if the magazine rotates clockwise (active only when the machine isin "JOG" mode)
Indicator on: The magazine rotates clockwise.
Indicator off: The magazine stops clockwise rotation.
Controls if the magazine approachesthe reference point(active onlywhen the machine isin "JOG"
mode)
LED on: The magazine is referenced.
LED off: The magazine is notyet referenced.
Controls if the magazine rotates counter-clockwise (active only when the machine is in "JOG" mode)
Indicator on: The magazine rotates counter-clockwise.
Indicator off: The magazine stops counter-clockwise rotation.
Controls if the chip remover rotates forward (active only when the machine is in "JOG" mode)
Indicator on: The chip remover starts forward rotation.
Indicator off: The chip remover stops rotation.
Controls if the chip remover rotates reversely (active only when the machine is in "JOG" mode)
Indicator on: The chip remover starts reverse rotation.
Indicator off: The chip remover stops reverse rotation.
K9 to K12 Reserved keys.
You can define the functions of these keys in PLC Programming Tool.For more information,see the
SINUMERIK 808D/SINUMERIK 808D ADVANCED Commissioning Manual.

Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017 15
Pre-defined labeling strips for keys of the MCP
The MCP package includes two sets (six pieces each) of pre-defined labeling strips.One set (①as shown below) is for the
turning variantof the control system and pre-inserted on the back of the MCP. The other set (②as shown below) is for the
milling variantofthe control system.
If your control system is a milling variantof the control system, replace the pre-inserted labeling stripswith the milling-
specific ones.
If the pre-defined labeling stripscannotmeetyourneeds,proceed as follows to make customized labeling stripsby using the
A4-sized blank plastic sheet in the MCP package:
1. Open the "Symbols for MCP customized key_808D"file in the "\examples\SINUMERIK_808D\MCP"folder on the
Toolbox DVD for the control system on your computer.
2. Copy the desired symbols of keys from the file and then paste them to the desired locations for key labelsin the
"Strip_template_808D"file.
3. Print the final labeling strip template file on the blank plastic sheet.
4. Replace the pre-inserted labeling stripsfrom the MCP with the customized ones.

Programming and Operating Manual (Milling)
16 6FC5398-4DP10-0BA6, 09/2017
2.3
Coordinate systems
As a rule, a coordinate system is formed from three mutually perpendicular coordinate axes.The positive directions of the
coordinate axes are defined using the Cartesian coordinate system.The coordinate system is related to the workpiece and
programming takes place independently ofwhetherthe tool or the workpiece is being traversed.When programming, it is
alwaysassumed thatthe tool traverses relative to the coordinate system of the workpiece,which is intended to be
stationary.
The figure below illustrateshow to determine the axis directions.
Machine coordinate system (MCS)
The orientation of the coordinate system relative to the machine dependson the respective machine types.It can be rotated
in differentpositions.
The directions of the axes follow the Cartesian coordinate system.
The figure below showsan example ofthe machine coordinate system ofa flat-body turning machine with a front tool holder.
The origin of this coordinate system is the
m achine zero
, defined by the machine manufacturer.
The traversing range of the
m achine axes
can be in the negative range.

Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017 17
Workpiece coordinate system (WCS)
To describe the geometryof a workpiece in the workpiece program, a right-handed,right-angled coordinate system is also
used.
Generally,X0/Y0 of the WCS is set at the center, edge or cornerof the workpiece while Z0 is set on the top surface of the
workpiece.
See the following illustrations for X0/Y0 at the center, edge and corner of the workpiece respectively.
The figure below shows an example ofthe workpiece coordinate system.
Relative coordinate system (REL)
In addition to the machine and workpiece coordinate systems,this control system providesa relative coordinate system.
This coordinate system can clear the current coordinate values atany position and has no influence on workpiece machining
or the position of WCS. All axis movements are displayed relative to this position.

Programming and Operating Manual (Milling)
18 6FC5398-4DP10-0BA6, 09/2017
2.4
Protection levels
Overview
The control system provides a concept of protection levelsfor enabling data areas.Differentprotection levels control
different access rights.
The control system delivered by Siemens is set by default to the lowestprotection level 7 (without password). If the
password is no longer known,the control system must be reinitialized with the default machine/drive data.All passwords are
then reset to defaultpasswords for this software release.
Note
Before you boot the control system with defaultmachine/drive data,make sure that you have backed up yourmachine/drive
data; otherwise,all data are lost after rebooting with default machine/drive data.
Protection level
Locked by
Area
0
Siemens password Siemens, reserved
1
Manufacturer password
Machine manufacturers
2
Reserved
-
3-6
End user password
(Default password: "CUSTOMER")
End users
7
No password End users
Protection level 1
Protection level 1 requires a manufacturerpassword.With this password entry, you can perform the following operations:
●Entering or changing partof the machine data and drive data
●Conducting NC and drive commissioning
Protection level 3-6
Protection level 3-6 requires an end user password.With this password entry, you can perform the following operations:
●Entering or changing partof the machine data
●Editing programs
●Setting offset values
●Measuring tools
Protection level 7
If you have not set the password or protection level interface signal,the system sets the protection level to 7 automatically.
With this password entry, you can perform the following operations:
●Editing programs
●Setting offset values
●Measuring tools
You can also set protection level 7 through the PLC user interfaces.For more information,see the
SINUMERIK 808D/SINUMERIK 808D ADVANCED Commissioning Manual.
In the menus listed below the inputand modification ofdata depends on the set protection level:
●Tool offsets
●Work offsets
●Setting data
●Program creation/program correction
The number ofmachine data and drive data which can be read or modified dependson the protection level.You can set the
protection level for these function areaswith the displaymachine data (
USER_CLASS
...).

Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017 19
Setting the password
+
1.
Select the system data operating area.
2.
Open the following password setting window and then enter the desired password (default
end
-user password: CUSTOMER):
3.
Confirm the input.
Changing/deleting the password
Note
To avoid unauthorized accessto the controller,you mustchange the Siemens defaultpasswords to yourown ones.
+
1.
Select the system data operating area.
2.
If you desire to change the existing password,press this softkey to open the following win-
dow and enterthe new password:
If you desire to delete the existing password,proceed directly to Step 6.
3.
Confirm the new password.
4.
Enter the new password again in the following window:
5.
Press this softkey to confirm the new password.
6.
If you desire to delete the existing password,directly press this softkey.

Programming and Operating Manual (Milling)
20 6FC5398-4DP10-0BA6, 09/2017
3
Common notices for machining operations
To ensure the safety and correctness of machining,you mustobserve the following noticesduring machining operations:
●Reference pointapproach is required only for machine tools equipped with incremental encoders.
●Before running the spindle manually,make sure you have activated the tool.
●Before executing M functions,make sure all the axes are in safe positions.
●During handwheel assignment,make sure there is no obstacle when moving the tool to avoid tool collision.
●To guarantee the safety and correctnessof machining,you mustverify the tool setup result.
●You mustdistinguish the direction of tool wear compensation clearlybefore entering the tool wear offsets.
●Before machining the workpiece on the machine,make sure the following preconditions are met:
–The PRT mode and the dry run feedrate are deactivated.
–The feedrate override is 0%.
–The safety door is closed.
●After changing importantdata,it is recommended to carry out an internal data backup immediately.
4
Switching on and referencing
Note
Reference pointapproach is required only for machine tools equipped with incremental encoders.
Operating sequence
1.
Turn on the power supplyfor the machine tool.
2.
Release all emergency stop buttons on the machine.By default, the control system is in
reference pointapproach (REF.POINT
) mode after startup.
•
If a machine axis isequipped with an absolute encoder,the axis is referenced
automatically after the control system starts and therefore reference point approach is
unnecessary.The circle symbol (lower-leftfigure) next to the axis
identifier indicates that
the axis is already referenced.
•
If a machine axis isequipped with an incremental encoder,the axis is not referenced
after the control system starts. The circle symbol (lower-rightfigure) next to the axis
identifier indicates that the axis has not been referenced.Proceed to Step 3.
3.
Use the corresponding axistraversing keys to traverse the axes until the symbol appears
next to the axis identifier.