Siemens SINUMERIK User manual

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

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

Programming and Operating Manual (Turning)
01/2017 3
Table of contents
Preface...................................................................................................................................................................2
1 Fundamental safety instructions ..............................................................................................................................7
1.1 General safety instructions......................................................................................................................7
1.2 Industrial security ....................................................................................................................................7
2 Introduction.............................................................................................................................................................8
2.1 Panel Processing Units (PPUs)...............................................................................................................8
2.1.1 PPU versions...........................................................................................................................................8
2.1.2 PPU control elements..............................................................................................................................9
2.1.3 Screen layout ........................................................................................................................................11
2.2 Machine Control Panels (MCPs) ...........................................................................................................12
2.2.1 MCP versions ........................................................................................................................................12
2.2.2 MCP control elements ...........................................................................................................................12
2.3 Coordinate systems...............................................................................................................................15
2.4 Protection levels ....................................................................................................................................16
3 Common notices for machining operations ............................................................................................................18
4 Switching on and referencing ................................................................................................................................18
5 Setting the user interface language ....................................................................................................................... 19
6 Setting up tools.....................................................................................................................................................20
6.1 Creating a tool.......................................................................................................................................20
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..................................................................................................................26
6.5.1 Measuring the tool manually (without the Y axis) ..................................................................................26
6.5.2 Measuring the tool manually (with the Y axis) .......................................................................................28
6.6 Verifying the tool offset result ................................................................................................................31
7 Creating part programs .........................................................................................................................................32
7.1 Creating a part program ........................................................................................................................32
7.2 Editing the part program........................................................................................................................34
7.2.1 Using a standard program structure......................................................................................................34
7.2.2 Editing a part program...........................................................................................................................34
7.2.3 Understanding frequently used programming instructions.....................................................................37
7.2.3.1 Dimension units in inch or mm (G70/G71).............................................................................................37
7.2.3.2 Definition of work offset (G54 to G59, G500, G90/G91) ........................................................................38
7.2.3.3 Rapid traverse (G00).............................................................................................................................39
7.2.3.4 Tool and traverse (T, D, F, G94/G95, S, M3/M4, G01)..........................................................................39
7.2.3.5 Tool radius compensation (G40, G41/G42)...........................................................................................39
7.2.3.6 Turning circles and arcs (G02/G03) ......................................................................................................40
7.2.3.7 Fixed point approach (G74/G75) ...........................................................................................................41
7.2.3.8 Spindle control.......................................................................................................................................41
7.2.3.9 Setting dwell time in the program (G04) ................................................................................................41
8 Program simulation...............................................................................................................................................42
8.1 Simulation prior to machining of the workpiece .....................................................................................42
8.2 Simultaneous recording prior to machining of the workpiece ................................................................44

Programming and Operating Manual (Turning)
401/2017
9 Machining the workpiece .......................................................................................................................................45
9.1 Executing a part program...................................................................................................................... 45
9.2 Executing specified blocks.................................................................................................................... 46
9.3 Correcting a part program..................................................................................................................... 47
9.4 Simultaneous recording during machining of the workpiece ................................................................. 47
9.5 Entering the tool wear offsets................................................................................................................ 48
10 Other common operations .....................................................................................................................................51
10.1 Program control functions ..................................................................................................................... 51
10.1.1 Program test ......................................................................................................................................... 51
10.1.2 Dry run feedrate .................................................................................................................................... 51
10.1.3 Conditional stop .................................................................................................................................... 52
10.1.4 Skip block.............................................................................................................................................. 52
10.1.5 Single block mode................................................................................................................................. 52
10.1.6 Rapid traverse override......................................................................................................................... 52
10.1.7 Auxiliary function lock............................................................................................................................ 52
10.2 Setting up the workpiece....................................................................................................................... 53
10.2.1 Measuring the workpiece ...................................................................................................................... 53
10.2.2 Entering/modifying workpiece offsets.................................................................................................... 54
10.3 Entering/modifying the setting data....................................................................................................... 55
10.4 Setting R parameters ............................................................................................................................ 58
10.5 Setting user data................................................................................................................................... 58
10.6 Setting the date and time ...................................................................................................................... 59
10.7 Executing/transferring a part program from external............................................................................. 59
10.7.1 Executing/transferring through the USB interface................................................................................. 59
10.7.1.1 Executing from external (through USB interface).................................................................................. 59
10.7.1.2 Transferring from external (through USB interface) .............................................................................. 60
10.7.2 Executing/transferring through the Ethernet connection ....................................................................... 61
10.7.2.1 Configuring the network drive ............................................................................................................... 61
10.7.2.2 Executing from external (through Ethernet connection) ........................................................................ 63
10.7.2.3 Transferring from external (through Ethernet connection)..................................................................... 64
10.7.3 Executing/transferring through the RS232 interface (PPU160.2 only) .................................................. 65
10.7.3.1 Configuring RS232 communication....................................................................................................... 65
10.7.3.2 Executing from external (through RS232 interface) .............................................................................. 66
10.7.3.3 Transferring from external (through RS232 interface)........................................................................... 67
10.7.4 Configuring the firewall.......................................................................................................................... 68
10.8 Extending/deactivating the CNC lock function ...................................................................................... 68
10.9 Data backup.......................................................................................................................................... 71
10.9.1 Internal data backup.............................................................................................................................. 71
10.9.2 External data backup ............................................................................................................................ 72
10.9.2.1 External data backup in a data archive ................................................................................................. 72
10.9.2.2 External data backup of separate files.................................................................................................. 73
10.10 Pocket calculator................................................................................................................................... 75
11 Programming principles.........................................................................................................................................76
11.1 Fundamentals of programming ............................................................................................................. 76
11.1.1 Program names .................................................................................................................................... 76
11.1.2 Program structure ................................................................................................................................. 77
11.2 Programming instructions ..................................................................................................................... 77
11.2.1 Programming dimensions ..................................................................................................................... 77
11.2.2 Absolute/incremental dimensioning: G90, G91, AC, IC......................................................................... 78
11.2.3 Dimensions in metric units and inches: G71, G70, G710, G700 ........................................................... 79
11.2.4 Radius/diameter dimensions: DIAMOF, DIAMON, DIAM90.................................................................. 79
11.2.5 Programmable work offset: TRANS, ATRANS...................................................................................... 81
11.2.6 Programmable scale factor: SCALE, ASCALE ..................................................................................... 83
11.2.7 Workpiece coordinate system- settable work offset: G54 to G59, G500, G53, G153 ........................... 84
11.3 Linear interpolation................................................................................................................................ 85

Programming and Operating Manual (Turning)
01/2017 5
11.3.1 Linear interpolation with rapid traverse: G0...........................................................................................85
11.3.2 Feedrate F.............................................................................................................................................86
11.3.3 Linear interpolation with feedrate: G1....................................................................................................87
11.4 Circular interpolation..............................................................................................................................87
11.4.1 Circular interpolation: G2, G3................................................................................................................87
11.4.2 Circular interpolation via intermediate point: CIP...................................................................................91
11.4.3 Circle with tangential transition: CT .......................................................................................................91
11.5 Thread cutting .......................................................................................................................................92
11.5.1 Thread cutting with constant lead: G33 .................................................................................................92
11.5.2 Programmable run-in and run-out path for G33: DITS, DITE ................................................................94
11.5.3 Thread cutting with variable lead: G34, G35 .........................................................................................95
11.5.4 Thread interpolation: G331, G332 .........................................................................................................96
11.6 Fixed point approach.............................................................................................................................97
11.6.1 Fixed point approach: G75 ....................................................................................................................97
11.6.2 Reference point approach: G74 ............................................................................................................97
11.7 Acceleration control and exact stop/continuous path ............................................................................98
11.7.1 Exact stop/continuous-path control mode: G9, G60, G64 .....................................................................98
11.7.2 Acceleration pattern: BRISK, SOFT ....................................................................................................100
11.7.3 Dwell Time: G4....................................................................................................................................100
11.8 The third axis.......................................................................................................................................101
11.9 Spindle movements.............................................................................................................................101
11.9.1 Spindle speed S, directions of rotation ................................................................................................101
11.9.2 Spindle positioning ..............................................................................................................................102
11.9.2.1 Spindle positioning (SPOS, SPOSA, M19, M70, WAITS)....................................................................102
11.9.2.2 Spindle positioning (SPOS, SPOSA, M19, M70, WAITS): Further information ...................................107
11.9.3 Gear stages.........................................................................................................................................108
11.10 Special turning functions .....................................................................................................................108
11.10.1 Constant cutting rate: G96, G97..........................................................................................................108
11.10.2 Rounding, chamfer ..............................................................................................................................110
11.10.3 Contour definition programming ..........................................................................................................112
11.11 Tool and tool offset..............................................................................................................................114
11.11.1 General information (turning)...............................................................................................................114
11.11.2 Tool T (turning)....................................................................................................................................114
11.11.3 Tool offset number D (turning).............................................................................................................115
11.11.4 Selecting the tool radius compensation: G41, G42 .............................................................................118
11.11.5 Corner behavior: G450, G451 .............................................................................................................120
11.11.6 Tool radius compensation OFF: G40...................................................................................................121
11.11.7 Special cases of the tool radius compensation....................................................................................121
11.11.8 Example of tool radius compensation (turning) ...................................................................................122
11.11.9 Special handling of tool compensation (turning)..................................................................................123
11.12 Miscellaneous function M ....................................................................................................................123
11.13 H function ............................................................................................................................................124
11.14 Arithmetic parameters, LUD and PLC variables..................................................................................124
11.14.1 Arithmetic parameter R........................................................................................................................124
11.14.2 Local User Data (LUD) ........................................................................................................................126
11.14.3 Reading and writing PLC variables .....................................................................................................127
11.15 Program jumps....................................................................................................................................127
11.15.1 Unconditional program jumps..............................................................................................................127
11.15.2 Conditional program jumps..................................................................................................................128
11.15.3 Program example for jumps ................................................................................................................129
11.15.4 Jump destination for program jumps ...................................................................................................130
11.16 Subroutine technique...........................................................................................................................131
11.16.1 General information.............................................................................................................................131
11.16.2 Calling machining cycles (turning).......................................................................................................132
11.16.3 Executing internal and external subroutines (CALL, EXTCALL)..........................................................133
11.17 Timers and workpiece counters...........................................................................................................134
11.17.1 Runtime timer......................................................................................................................................134
11.17.2 Workpiece counter...............................................................................................................................136
11.18 Kinematic transformation.....................................................................................................................138
11.18.1 Face milling on turned parts (TRANSMIT)...........................................................................................138
11.18.2 Cylinder surface transformation (TRACYL) .........................................................................................140

Programming and Operating Manual (Turning)
601/2017
12 Cycles ................................................................................................................................................................147
12.1 Overview of cycles .............................................................................................................................. 147
12.2 Programming cycles............................................................................................................................ 147
12.3 Graphical cycle programming in the program editor............................................................................ 148
12.4 Drilling cycles ...................................................................................................................................... 149
12.4.1 General information............................................................................................................................. 149
12.4.2 Requirements...................................................................................................................................... 150
12.4.3 Drilling, centering - CYCLE81 ............................................................................................................. 152
12.4.4 Drilling, counterboring - CYCLE82 ...................................................................................................... 154
12.4.5 Deep-hole drilling - CYCLE83 ............................................................................................................. 156
12.4.6 Rigid tapping - CYCLE84 .................................................................................................................... 160
12.4.7 Tapping with compensating chuck - CYCLE840................................................................................. 164
12.4.8 Reaming1 - CYCLE85......................................................................................................................... 168
12.4.9 Boring - CYCLE86............................................................................................................................... 170
12.5 Turning cycles..................................................................................................................................... 172
12.5.1 Requirements...................................................................................................................................... 172
12.5.2 Cutoff - CYCLE92 ............................................................................................................................... 174
12.5.3 Groove - CYCLE93 ............................................................................................................................. 176
12.5.4 Undercut (forms E and F to DIN) - CYCLE94 ..................................................................................... 183
12.5.5 Cutting with relief cut - CYCLE95........................................................................................................ 186
12.5.6 Thread undercut - CYCLE96............................................................................................................... 200
12.5.7 Thread chaining - CYCLE98 ............................................................................................................... 203
12.5.8 Thread cutting - CYCLE99 .................................................................................................................. 208
12.6 Error messages and error handling..................................................................................................... 215
12.6.1 General Information ............................................................................................................................ 215
12.6.2 Error handling in the cycles................................................................................................................. 215
12.6.3 Overview of cycle alarms .................................................................................................................... 215
12.6.4 Messages in the cycles....................................................................................................................... 215
13 Machining typical turning parts.............................................................................................................................216
13.1 Operations before programming ......................................................................................................... 216
13.2 Programming for machining a spherical surface (Example 1)............................................................. 216
13.3 Programming for machining contours (Example 2) ............................................................................. 221
13.4 Programming for roughing, grooving and threading (Example 3)........................................................ 228
13.5 Programming for roughing and finishing (Example 4) ......................................................................... 236
13.6 Program simulation and execution...................................................................................................... 242
A Appendix ............................................................................................................................................................243
A.1 Operating area overview..................................................................................................................... 243
A.1.1 Machining operating area.................................................................................................................... 243
A.1.2 Program editing operating area........................................................................................................... 243
A.1.3 Offset operating area .......................................................................................................................... 244
A.1.4 Program management operating area ................................................................................................ 245
A.1.5 System data operating area................................................................................................................ 249
A.1.6 Alarm operating area........................................................................................................................... 250
A.2 Operating mode overview ................................................................................................................... 251
A.2.1 "AUTO" mode...................................................................................................................................... 251
A.2.2 "JOG" mode ........................................................................................................................................ 252
A.2.2.1 Running the spindle manually ............................................................................................................. 254
A.2.2.2 Executing M functions......................................................................................................................... 255
A.2.2.3 Setting the relative coordinate system (REL)...................................................................................... 255
A.2.2.4 Setting the JOG data........................................................................................................................... 256
A.2.3 "MDA" mode........................................................................................................................................ 257
A.3 Additional method for measuring the tool............................................................................................ 258
A.4 Activating the contour handwheel via the NC program ....................................................................... 259
A.5 The help system.................................................................................................................................. 261
A.6 Operation wizard................................................................................................................................. 263
A.7 Editing Chinese characters ................................................................................................................. 264
A.8 Calculating contour elements.............................................................................................................. 265

Programming and Operating Manual (Turning)
01/2017 7
A.9 Free contour programming..................................................................................................................269
A.9.1 Defining a start point............................................................................................................................271
A.9.2 Programming contour element ............................................................................................................272
A.9.3 Parameters for contour elements ........................................................................................................275
A.9.4 Undercuts for turning technology.........................................................................................................278
A.9.5 Specifying contour elements in polar coordinates ...............................................................................278
A.9.6 Cycle support ......................................................................................................................................281
A.9.7 Programming example for turning application .....................................................................................281
A.10 Word structure and address ................................................................................................................285
A.11 Character set.......................................................................................................................................286
A.12 Block format ........................................................................................................................................287
A.13 List of instructions................................................................................................................................288
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 associate
d hardware documentation are not observed, accidents involving
severe injuries or death can occur.
•Observe the safety instructions given in the hardware documentation.
•
Consider the residual risks for the risk evaluation.
WARNING
Danger to life or malfunctions of the machine as a result of incorrect or changed parameterization
As a result of incorrect or changed parameterization, machines can malfunction, which in turn can lead to injuries or death.
•Protect the parameterization (parameter assignments) against unauthorized access.
•
Respond to possible malfunctions by applying suitable measures (e.g. EMERGENCY STOP or EMERGENCY OFF).
1.2
Industrial security
Note
Industrial security
Siemens provides products and solutions with industrial security functions that support the secure operation of plants,
systems, machi
nes and networks.
In order to protect plants, systems, machines and networks against cyber threats, it is necessary to implement
– and
continuously maintain
– a holistic, state-of-the-art industrial security concept. Siemens products and solutions only rep
resent
one component of such a concept.
The customer is responsible for preventing unauthorized access to its plants, systems, machines and networks. Systems,
machines and components should only be connected to the enterprise network or the internet if and
to the extent necessary
and with appropriate security measures (e.g. use of firewalls and network segmentation) in place.
Additionally, Siemens’ guidance on appropriate security measures should be taken into account. For more information about
industrial
security, please visit:
Industrial security (
http://www.siemens.com/industrialsecurity).
Siemens’ products and solutions undergo continuous development to make them more secure. Siemens strongly
r
ecommends to apply product updates as soon as available and to always use the latest product versions. Use of product
versions that are no longer supported, and failure to apply latest updates may increase customer’s exposure to cyber
threats.
To stay inf
ormed about product updates, subscribe to the Siemens Industrial Security RSS Feed at:
Industrial security (
http://www.siemens.com/industrialsecurity).

Programming and Operating Manual (Turning)
801/2017
WARNING
Danger to life as a result of unsafe operating states resulting from software manipulation
Software manipulations (e.g. viruses, trojans, malware or worms) can cause unsafe operating states in your system that
may lead to death, serious injury, and property damage.
•Keep the software up to date.
•Incorporate the automation and drive components into a holistic, state-of-the-art industrial security concept for the
installation or machine.
•Make sure that you include all installed products into the holistic industrial security concept.
•Protect files stored on exchangeable storage media from malicious software by with suitable protection measures, e.g.
virus scanners.
2
Introduction
Note
Chapter "
Machining typical turning parts (Page 216)" 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
PPU versions
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
PPU160.2 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
PPU141.2 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

Programming and Operating Manual (Turning)
01/2017 9
2.1.2
PPU control elements
①
Status indicators
⑧
Alarm cancellation key
Cancels alarms and messages that are 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
USB 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 (Turning)
10 01/2017
Additional information about keys
<CTRL + P>: Creates a screenshot of the actual user interface
<CTRL + S>: Saves startup archives and action logs to a USB stick
<CTRL + D>: Displays pre-defined slides on the screen
<ALT + D>: Saves action logs to a USB stick
Calls the calculator function when you position the cursor on the desired input field
<CTRL + cursor key>: Changes the screen backlight brightness by an increment of 10% (bright-
ness range: 10% to 100%)
Note that after you release the key combination, the HMI saves your brightness setting and the
brightness bar disappears after a few seconds.
The graphical symbols shown on the six keys above are available only on the PPU161.3 and
PPU160.2.
Enters the upper character shown on the alphabetic/numeric keys concerned
+
Opens the system data operating area
In the program editor, pressing this key moves the cursor to the beginning of the 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, for example, generation of user dialog boxes with
the EasyXLanguage function. For more information about this function, see the SINUMERIK
808D/SINUMERIK 808D ADVANCED Function Manual.
Status indicators
Indicator
Status and meaning
"POK"
•
Solid green: The power supply 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 of the control system is within the specified scope.
•
Solid orange: The temperature of the control system is beyond the scope.

Programming and Operating Manual (Turning)
01/2017 11
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 lettering on a red
background. The associated alarm text is shown in red letter-
ing. An arrow indicates that several alarms are active. The
number to the right of the arrow indicates the total number of
active alarms. When more than one alarm is active, the dis-
play scrolls through the alarms in sequence. An acknowl-
edgement symbol indicates the alarm cancel criterion.
Displays messages from NC programs
Messages from NC programs do not have numbers and ap-
pear in green lettering.

Programming and Operating Manual (Turning)
12 01/2017
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 switch-
es
•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 any of the following con-
trol systems:
•SINUMERIK 808D ADVANCED T (Turning)
•SINUMERIK 808D ADVANCED M (Milling)
•SINUMERIK 808D (Turning)
•SINUMERIK 808D (Milling)
•Horizontal MCP, with Chinese keys and a reserved slot
for the handwheel This MCP variant is applicable to the following control sys-
tems:
•SINUMERIK 808D ADVANCED T (Turning)
•
SINUMERIK 808D (Turning)
2.2.2
MCP control elements
Horizontal MCP
•
Variant with override switches
•
Variant with a reserved slot for the handwheel

Programming and Operating Manual (Turning)
01/2017 13
Vertical MCP
•Variant with an override switch for the spindle •Variant with a reserved slot for the handwheel
①Reserved hole for emergency stop button ⑨Spindle control keys
②Tool number display
Displays the number of the currently active tool
⑩Keys for program start, stop, and reset
③Operating mode selection area ⑪Pre-defined labeling strips for keys of the MCP
④Program control keys ⑫Reserved slot for the handwheel
⑤User-defined keys ⑬Spindle override control keys
⑥Axis traversing keys ⑭Feedrate override control keys
⑦Spindle override switch ⑮Keys for increment override/rapid traverse override*
⑧Feedrate override switch
* The increment override can be activated in "JOG" mode, "Handwheel" mode, or "AUTO"/"MDA" mode with the contour
handwheel activated. The rapid traverse override is effective only in "AUTO"/"MDA" mode with no contour handwheel ac-
tivated. The "F0 G00" key can activate a rapid traverse override of 1% by default, which can be changed in the general
machine data 12050[1], for example, 12050[1] = 0.15 as 15%.
Functions of user-defined keys
Switches on/off the machine tool working lamp (always active independent of the 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 coolant supply (always active independent of the machine operating mode)
Indicator on: The coolant supply is switched on.
Indicator off: The coolant supply is switched off.
Enables/disables the sequential tool changes (active only when the machine is in "JOG" mode)
Indicator on: The machine starts sequential tool changes.
Indicator off: The machine stops sequential tool changes.
Controls the clamping/unclamping of the workpiece by the chuck (active only when the machine is in "JOG"
mode and the spindle has stopped running)
Indicator on: The chuck has clamped the workpiece.
Indicator off: The chuck has unclamped the workpiece.
Controls the internal/external clamping of the workpiece by the chuck (active only when the spindle has
stopped running)
Indicator on: The chuck has clamped the workpiece externally.
Indicator off: The chuck has clamped the workpiece internally.

Programming and Operating Manual (Turning)
14 01/2017
Enables/disables the tailstock to hold the workpiece tightly (active only when the machine is in "JOG" mode)
Indicator on: The tailstock moves towards the workpiece until it holds the workpiece tightly.
Indicator off: The tailstock retracts from the workpiece to its original position.
K1 to K5,
K7 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.
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 variant of the control system and pre-inserted on the back of the MCP. The other set (②as shown below) is for the
milling variant of the control system.
Note
For the horizontal MCP variant with a reserved slot for the handwheel, no pre
-defined labeling strip is provided.
If your control system is a milling variant of the control system, replace the pre-inserted labeling strips with the milling-
specific ones.
If the pre-defined labeling strips cannot meet your needs, proceed as follows to make customized labeling strips by using the
A4-sized blank plastic sheet in the MCP package:
1. Open the "Symbols for MCP customized key_808D" file in one of the following folders on the Toolbox DVD for the control
system on your computer:
–\examples\SINUMERIK_808D\MCP (for PPU141.2)
–\examples\SINUMERIK_808D_ADVANCED\MCP (for PPU160.2 and PPU161.3)
2. Copy the desired symbols of keys from the file and then paste them to the desired locations for key labels in the
"Strip_template_808D" file.
3. Print the final labeling strip template file on the blank plastic sheet.
4. Replace the pre-inserted labeling strips from the MCP with the customized ones.
Note
The MCP information described in this manual is valid for the SINUMERIK 808D MCP.

Programming and Operating Manual (Turning)
01/2017 15
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 of whether the tool or the workpiece is being traversed. When programming, it is
always assumed that the tool traverses relative to the coordinate system of the workpiece, which is intended to be
stationary.
The figure below illustrates how to determine the axis directions.
Machine coordinate system (MCS)
The orientation of the coordinate system relative to the machine depends on the machine type. It can be rotated in different
positions.
The directions of the axes follow the Cartesian coordinate system. Seen from the front of the machine, the middle finger of
the right hand points in the opposite direction to the infeed of the spindle.
The figure below shows an example of the machine coordinate system of a flat-body turning machine with a front tool holder.
The origin of this coordinate system is the machine zero, defined by the machine manufacturer.

Programming and Operating Manual (Turning)
16 01/2017
Workpiece coordinate system (WCS)
WCS refers to the coordinate system which is used to describe the geometry of a workpiece in the workpiece program.
The origin of the coordinate system: the X axis is set at the rotating center of the workpiece while the Z axis is set at the
surface of the workpiece.
Relative coordinate system (REL)
In addition to the machine and workpiece coordinate systems, the control system provides a relative coordinate system. This
coordinate system can clear the current coordinate values at any position and has no influence on workpiece machining or
the position of WCS. All axis movements are displayed relative to this position.
2.4
Protection levels
Overview
The control system provides a concept of protection levels for enabling data areas. Different protection levels control
different access rights.
The control system delivered by Siemens is set by default to the lowest protection 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 default passwords for this software release.
Note
Before you boot the control system with default machine/drive data, make sure that you have backed up your machine/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 manufacturer password. With this password entry, you can perform the following operations:
●Entering or changing part of 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 part of 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.

Programming and Operating Manual (Turning)
01/2017 17
In the menus listed below the input and modification of data depends on the set protection level:
●Tool offsets
●Work offsets
●Setting data
●Program creation/program correction
The number of machine data and drive data which can be read or modified depends on the protection level. You can set the
protection level for these function areas with the display machine data (
USER_CLASS
...).
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 access to the controller, you must change the Siemens default passwords to yo
ur own ones.
+
1.
Select the system data operating area.
2.
If you desire to change the existing password, press this softkey to open the foll
owing win-
dow and enter the 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:

Programming and Operating Manual (Turning)
18 01/2017
5.
Press this softkey to confirm the new password.
6.
If you desire to delete the existing password, directly press this softkey.
3
Common notices for machining operations
To ensure the safety and correctness of machining, you must observe the following notices during machining operations:
●Reference point approach 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 correctness of machining, you must verify the tool setup result.
●You must distinguish the direction of tool wear compensation clearly before 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 important data, it is recommended to carry out an internal data backup immediately.
4
Switching on and referencing
Note
Reference
point approach is required only for machine tools equipped with incremental encoders.
Operating sequence
1.
Turn on the power supply for the machine tool.
2.
Release all emergency stop buttons on the machi
ne. By default, the control system is in
reference point approach (REF.POINT) mode after startup.
•
If a machine axis is equipped 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-
left figure) next to the axis identifier indicates that
the axis is already referenced.
•
If a machine axis is equipped with an incremental encoder, the axis is not referenced
after the control system starts. The circle symbol (lower-right figure) next to the axis
identifier indicates that the axis has not been referenced. Proceed to Step 3.

Programming and Operating Manual (Turning)
01/2017 19
3.
Use the corresponding axis traversing keys to traverse
the axes until the
symbol appears
next to the axi
s identifier.
5
Setting the user interface language
Note
The default user interface language is dependent on the PPU type. For a PPU with Chinese keys, the default language is
Chinese after power
-on; otherwise it's English. If you desire to change it, p
roceed through the following operating sequence;
otherwise, skip this chapter and proceed to the next chapter for setting up tools.
Operating sequence
+
1.
Select the system data operating area.
2.
Open the user interface language selection window.
3.
Use the cursor keys to select the desired language.
4.
Press this softkey to confirm your selection and the system is automatically restarted to
activate the selected language.

Programming and Operating Manual (Turning)
20 01/2017
6
Setting up tools
6.1
Creating a tool
Note
The control system supports a maximum of 64 tools and 128 cutting edges
. You can create a maximum of nine cutting
edges for each tool. Before executing a part program, you must first create the desired tool in the tool list and proceed wit
h
the tool setting operations.
Operating sequence
1.
Select the offset operating area.
2.
Open the tool list window.
3.
Open the lower
-level menu for tool type selection.
4.
Select a tool type (for example, a turning tool) with the corresponding softkey.
5.
Enter the tool num
ber and then select the corresponding tool edge position code in the
following window according to the actual tool tip direction, the actual positive directions of
the machine axes X and Z, as well as the description about tool edge positions given in the
illustration under the screenshot below.