Siemens SINUMERIK 808D User manual

© Siemens AG 2015. All rights reserved
6FC5398-5DP10-0BA2, 06/2015 1
SINUMERIK
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)
26FC5398-5DP10-0BA2, 06/2015
Preface
Applicable software versions for turning
Applicable products
This manual is applicable to the following control system:
Control system
Software version
SINUMERIK 808D ADVANCED T (Turning) V4.7
Preface
Documentation components and target groups
Document
Recommended target group
Programming and Operating Manual (Turning) Programmers and operators of turning machines
Programming and Operating Manual (Milling) Programmers and operators of milling machines
Diagnostics Manual Mechanical and electrical designers, commissioning engi-
neers, machine operators, and service and maintenance
personnel
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:
•Global Web site:
https://support.industry.siemens.com/sc/us/en/sc/list-of-countries/oid2044
•Chinese Web site:
http://www.siemens.com.cn/808D
Germany [phone]
China [phone]
1) You can find more hotline information at the global 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)
6FC5398-5DP10-0BA2, 06/2015 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 CNC operator panels...............................................................................................................................8
2.1.1 Panel Processing Unit (PPU) versions ....................................................................................................8
2.1.2 Control elements on the PPU161.3 .........................................................................................................8
2.2 Machine control panels..........................................................................................................................10
2.2.1 Machine Control Panel (MCP) versions.................................................................................................10
2.2.2 Control elements on the MCP ...............................................................................................................10
2.3 Screen layout ........................................................................................................................................12
2.4 Protection levels ....................................................................................................................................13
2.5 Setting user interface language.............................................................................................................14
3 Turning on, reference point approach ....................................................................................................................15
4 Setting-up.............................................................................................................................................................16
4.1 Coordinate systems...............................................................................................................................16
4.2 Setting up tools......................................................................................................................................18
4.2.1 Creating a new tool................................................................................................................................18
4.2.2 Activating the tool..................................................................................................................................20
4.2.3 Assigning the handwheel.......................................................................................................................21
4.2.4 Activating the spindle.............................................................................................................................22
4.2.5 Measuring the tool (manually) ...............................................................................................................23
4.2.6 Verifying the tool offset result in "MDA" mode.......................................................................................27
4.2.7 Entering/modifying the tool wear data ...................................................................................................28
4.3 Operating area overview .......................................................................................................................29
5 Part programming .................................................................................................................................................30
5.1 Creating a part program ........................................................................................................................31
5.2 Editing part programs ............................................................................................................................31
5.3 Managing part programs .......................................................................................................................33
6 Automatic machining.............................................................................................................................................36
6.1 Simulating machining ............................................................................................................................37
6.1.1 Simulation prior to machining of the workpiece .....................................................................................37
6.1.2 Simultaneous recording prior to machining of the workpiece ................................................................39
6.1.3 Simultaneous recording during machining of the workpiece..................................................................39
6.2 Program control.....................................................................................................................................40
6.3 Program test..........................................................................................................................................41
6.4 Starting and stopping/interrupting a part program .................................................................................43
6.5 Executing/transferring a part program through the Ethernet connection ...............................................44
6.5.1 Configuring the network drive................................................................................................................44
6.5.2 Executing from external (through Ethernet connection).........................................................................46
6.5.3 Transferring from external (through Ethernet connection).....................................................................47
6.6 Machining at a specific point .................................................................................................................48
7 Data backup .........................................................................................................................................................49
7.1 Internal data backup..............................................................................................................................49

Programming and Operating Manual (Turning)
46FC5398-5DP10-0BA2, 06/2015
7.2 External data backup ............................................................................................................................ 50
7.2.1 External data backup in a data archive ................................................................................................. 50
7.2.2 Exernal data backup of separate files ................................................................................................... 52
8 Programming principles.........................................................................................................................................53
8.1 Fundamentals of programming ............................................................................................................. 53
8.1.1 Program names .................................................................................................................................... 53
8.1.2 Program structure ................................................................................................................................. 53
8.2 Positional data ...................................................................................................................................... 53
8.2.1 Programming dimensions ..................................................................................................................... 53
8.2.2 Absolute/incremental dimensioning: G90, G91, AC, IC......................................................................... 54
8.2.3 Dimensions in metric units and inches: G71, G70, G710, G700 ........................................................... 55
8.2.4 Radius/diameter dimensions: DIAMOF, DIAMON, DIAM90.................................................................. 56
8.2.5 Programmable work offset: TRANS, ATRANS...................................................................................... 56
8.2.6 Programmable scaling factor: SCALE, ASCALE................................................................................... 59
8.2.7 Workpiece clamping - settable work offset: G54 to G59, G500, G53, G153 ......................................... 60
8.2.8 Kinematic transformation ...................................................................................................................... 61
8.2.8.1 Milling on turned parts (TRANSMIT) ..................................................................................................... 61
8.2.8.2 Cylinder surface transformation (TRACYL)........................................................................................... 63
8.3 Linear interpolation................................................................................................................................ 69
8.3.1 Linear interpolation with rapid traverse: G0........................................................................................... 69
8.3.2 Feedrate F ............................................................................................................................................ 70
8.3.3 Linear interpolation with feedrate: G1 ................................................................................................... 71
8.4 Circular interpolation ............................................................................................................................. 71
8.4.1 Circular interpolation: G2, G3................................................................................................................ 71
8.4.2 Circular interpolation via intermediate point: CIP .................................................................................. 74
8.4.3 Circle with tangential transition: CT....................................................................................................... 75
8.5 Thread cutting ....................................................................................................................................... 75
8.5.1 Thread cutting with constant lead: G33................................................................................................. 75
8.5.2 Programmable run-in and run-out path for G33: DITS, DITE................................................................ 78
8.5.3 Thread cutting with variable lead: G34, G35......................................................................................... 79
8.5.4 Thread interpolation: G331, G332......................................................................................................... 80
8.6 Fixed point approach............................................................................................................................. 81
8.6.1 Fixed point approach: G75.................................................................................................................... 81
8.6.2 Reference point approach: G74 ............................................................................................................ 81
8.7 Acceleration control and exact stop/continuous path ............................................................................ 82
8.7.1 Exact stop/continuous-path control mode: G9, G60, G64..................................................................... 82
8.7.2 Acceleration pattern: BRISK, SOFT...................................................................................................... 84
8.7.3 Dwell Time: G4 ..................................................................................................................................... 84
8.8 The third axis ........................................................................................................................................ 85
8.9 Spindle movements............................................................................................................................... 85
8.9.1 Spindle speed S, directions of rotation.................................................................................................. 85
8.9.2 Spindle positioning................................................................................................................................ 86
8.9.2.1 Spindle positioning (SPOS, SPOSA, M19, M70, WAITS)..................................................................... 86
8.9.2.2 Spindle positioning (SPOS, SPOSA, M19, M70, WAITS): Further information..................................... 90
8.9.3 Gear stages .......................................................................................................................................... 92
8.10 Special turning functions....................................................................................................................... 92
8.10.1 Constant cutting rate: G96, G97 ........................................................................................................... 92
8.10.2 Rounding, chamfer................................................................................................................................ 93
8.10.3 Contour definition programming............................................................................................................ 96
8.11 Tool and tool offset................................................................................................................................ 97
8.11.1 General information (turning) ................................................................................................................ 97
8.11.2 Tool T (turning) ..................................................................................................................................... 98
8.11.3 Tool offset number D (turning) .............................................................................................................. 98
8.11.4 Selecting the tool radius compensation: G41, G42............................................................................. 101
8.11.5 Corner behavior: G450, G451............................................................................................................. 103
8.11.6 Tool radius compensation OFF: G40 .................................................................................................. 103
8.11.7 Special cases of the tool radius compensation ................................................................................... 104
8.11.8 Example of tool radius compensation (turning)................................................................................... 105
8.11.9 Special handling of tool compensation (turning) ................................................................................. 105

Programming and Operating Manual (Turning)
6FC5398-5DP10-0BA2, 06/2015 5
8.12 Miscellaneous function M ....................................................................................................................106
8.13 H function ............................................................................................................................................107
8.14 Arithmetic parameters, LUD and PLC variables..................................................................................107
8.14.1 Arithmetic parameter R........................................................................................................................107
8.14.2 Local User Data (LUD) ........................................................................................................................108
8.14.3 Reading and writing PLC variables .....................................................................................................109
8.15 Program jumps....................................................................................................................................110
8.15.1 Unconditional program jumps..............................................................................................................110
8.15.2 Conditional program jumps..................................................................................................................111
8.15.3 Program example for jumps ................................................................................................................112
8.15.4 Jump destination for program jumps ...................................................................................................113
8.16 Subroutine technique...........................................................................................................................113
8.16.1 General information.............................................................................................................................113
8.16.2 Calling machining cycles (turning).......................................................................................................115
8.16.3 Executing external subroutines (EXTCALL) ........................................................................................115
8.17 Timers and workpiece counters...........................................................................................................116
8.17.1 Runtime timer......................................................................................................................................116
8.17.2 Workpiece counter...............................................................................................................................118
9 Cycles ................................................................................................................................................................ 119
9.1 Overview of cycles...............................................................................................................................119
9.2 Programming cycles............................................................................................................................120
9.3 Graphical cycle support in the program editor.....................................................................................121
9.4 Drilling cycles ......................................................................................................................................122
9.4.1 General information.............................................................................................................................122
9.4.2 Requirements ......................................................................................................................................122
9.4.3 Drilling, centering - CYCLE81..............................................................................................................125
9.4.4 Drilling, counterboring - CYCLE82.......................................................................................................127
9.4.5 Deep-hole drilling - CYCLE83 .............................................................................................................129
9.4.6 Rigid tapping - CYCLE84 ....................................................................................................................133
9.4.7 Tapping with compensating chuck - CYCLE840 .................................................................................137
9.4.8 Reaming1 - CYCLE85.........................................................................................................................141
9.4.9 Boring - CYCLE86...............................................................................................................................143
9.5 Turning cycles .....................................................................................................................................145
9.5.1 Requirements ......................................................................................................................................145
9.5.2 Cutoff - CYCLE92................................................................................................................................147
9.5.3 Groove - CYCLE93..............................................................................................................................149
9.5.4 Undercut (forms E and F to DIN) - CYCLE94......................................................................................156
9.5.5 Cutting with relief cut - CYCLE95 ........................................................................................................159
9.5.6 Thread undercut - CYCLE96...............................................................................................................173
9.5.7 Thread chaining - CYCLE98................................................................................................................176
9.5.8 Thread cutting - CYCLE99 ..................................................................................................................181
9.6 Error messages and error handling .....................................................................................................188
9.6.1 General Information.............................................................................................................................188
9.6.2 Error handling in the cycles .................................................................................................................188
9.6.3 Overview of cycle alarms.....................................................................................................................188
9.6.4 Messages in the cycles .......................................................................................................................188
10 Typical turning programs..................................................................................................................................... 189
A Appendix ............................................................................................................................................................ 194
A.1 Creating a new cutting edge................................................................................................................194
A.2 Setting up the workpiece .....................................................................................................................195
A.2.1 Measuring the workpiece.....................................................................................................................195
A.2.2 Entering/modifying work offsets...........................................................................................................197
A.3 Entering/modifying the setting data .....................................................................................................197
A.4 Setting R parameters...........................................................................................................................201
A.5 Setting user data .................................................................................................................................202

Programming and Operating Manual (Turning)
66FC5398-5DP10-0BA2, 06/2015
A.6 Other settings in "JOG" mode ............................................................................................................. 202
A.6.1 Setting the relative coordinate system (REL)...................................................................................... 204
A.6.2 Setting the JOG data........................................................................................................................... 204
A.7 Activating the contour handwheel via the NC program ....................................................................... 205
A.8 Notes on part programs in "MDA" mode ............................................................................................. 207
A.9 The help system.................................................................................................................................. 207
A.10 Operation wizard................................................................................................................................. 210
A.11 Editing Chinese characters ................................................................................................................. 211
A.12 Pocket calculator................................................................................................................................. 212
A.13 Calculating contour elements.............................................................................................................. 213
A.14 Free contour programming.................................................................................................................. 217
A.14.1 Programming a contour....................................................................................................................... 219
A.14.2 Defining a start point ........................................................................................................................... 219
A.14.3 Programming contour element............................................................................................................ 220
A.14.4 Parameters for contour elements........................................................................................................ 223
A.14.5 Undercuts for turning technology ........................................................................................................ 226
A.14.6 Specifying contour elements in polar coordinates............................................................................... 226
A.14.7 Cycle support...................................................................................................................................... 229
A.14.8 Programming example for turning application..................................................................................... 229
A.15 Word structure and address................................................................................................................ 233
A.16 Character set ...................................................................................................................................... 234
A.17 Block format........................................................................................................................................ 235
A.18 List of instructions ............................................................................................................................... 236

Programming and Operating Manual (Turning)
6FC5398-5DP10-0BA2, 06/2015 7
1
Fundamental safety instructions
1.1
General safety instructions
WARNING
Risk of death if the safety instructions and remaining risks are not carefully observed
If the safety instructions and residual risks are not observed in the associated hardware documentation, 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,
solutions, machines, equipment and/or networks. They are important components in a holistic industrial security concept.
With this in mind, Siemens’ products and solutions undergo continuous development. Siemens recommends strongly that
you regularly check for product updates.
For the secure operation of Siemens products and solutions, it is necessary to take suitable preventive action (e.g. cell
protection concept) and integrate each component into a holistic, state-of-the-art industrial security concept. Third-party
products that may be in use should also be considered. For more information about industrial security, visit this address
(http://www.siemens.com/industrialsecurity).
To stay informed about product updates as they occur, sign up for a product-specific newsletter. For more information, visit
this address (http://support.automation.siemens.com).
WARNING
Danger as a result of unsafe operating states resulting from software manipulation
Software manipulation (e.g. by viruses, Trojan horses, malware, worms) can cause unsafe operating states to develop in
your installation which can result in death, severe injuries and/or material damage.
•Keep the software up to date.
You will find relevant information and newsletters at this address (http://support.automation.siemens.com).
•Incorporate the automation and drive components into a holistic, state-of-the-art industrial security concept for the
installation or machine.
You will find further information at this address (http://www.siemens.com/industrialsecurity).
•Make sure that you include all installed products into the holistic industrial security concept.

Programming and Operating Manual (Turning)
86FC5398-5DP10-0BA2, 06/2015
2
Introduction
2.1
CNC operator panels
2.1.1
Panel Processing Unit (PPU) versions
PPU version
Panel layout
Applicable control system
PPU161.3 Horizontal, English version SINUMERIK 808D ADVANCED T (Turning)/M (Milling)
Horizontal, Chinese version
2.1.2
Control elements on the PPU161.3
①
Vertical and horizontal softkeys
Calls specific menu functions
②
Return key
Returns to the next higher-level menu
③
Menu extension key
Opens the next lower-level menu or navigate between the menus of the same level
④
Alphabetic and numeric keys
⑤
Control keys
⑥
Alarm cancellation key
Cancels alarms and messages that are marked with this symbol
⑦
On-board wizard key
Provides step-by-step guides on basic commissioning and operation procedures
⑧
Help key
Calls help information
⑨
Cursor keys
⑩
Operating area keys
⑪
USB interface
⑫
Status LEDs

Programming and Operating Manual (Turning)
6FC5398-5DP10-0BA2, 06/2015 9
Keys with icons
The icon on the key is a hint that you can press both <CTRL> and this key as shortcuts for capturing
screens.
The icon on the key is a hint that you can press both <CTRL> and this key as shortcuts for saving
start-up archives and action logs to a USB stick.
The icon on the key is a hint that you can press both <CTRL> and this key as shortcuts for displaying
pre-defined slides on the screen or both <ALT> and this key as shortcuts for saving action logs to a
USB stick.
The icon on the key is a hint that you can press this key to call the calculator function.
The icon on the key is a hint that this key can be used together with another key to function as a key
combination.
Further information
To enter the upper character on an alphabetic/numeric/operating area key, keep this key pressed.
•Toggles between entries in the input field
•Enters the "Set-up menu" dialog at NC start-up
To open the system data management operating area, press the following key combination:
+
Enables user-defined extension applications, for example, generation of user dialogs with the
EasyXLanguage function.
For more information about this function, see the SINUMERIK 808D/SINUMERIK 808D ADVANCED
Function Manual.
USB interface Connects to a USB device, for example:
•An external USB memory stick, to transfer data between the USB stick and the CNC
•An external USB keyboard which functions as an external NC keyboard
Status LEDs
LED "POK" Solid green: The power supply for the CNC is switched on.
LED "RDY" •Solid green: The CNC is ready and the PLC is in running mode.
•Solid red: The CNC is in stop mode.
•Solid orange: The PLC is in stop mode.
•Flashing orange: The PLC is in power-up mode.
LED "TEMP" •Off: The CNC temperature is within the specified range.
•Solid orange: The CNC temperature is out of range.
Backlight brightness control
Pressing <CTRL> and the cursor keys sets the screen backlight brightness by an increment of 10%
(brightness range: 10% to 100%).
Note that after you release the key combination, the HMI saves your brightness settings and the
brightness bar disappears after three seconds.

Programming and Operating Manual (Turning)
10 6FC5398-5DP10-0BA2, 06/2015
2.2
Machine control panels
2.2.1
Machine Control Panel (MCP) versions
MCP version
Applicable control system
•Horizontal MCP, English version
•Horizontal MCP, Chinese version
•Vertical MCP with a reserved slot for the handwheel, English version
•Vertical MCP with a reserved slot for the handwheel, Chinese version
•Vertical MCP with an override switch for the spindle, English version
•
Vertical MCP with an override switch for the spindle, Chinese version
SINUMERIK 808D ADVANCED T (Turning)/M
(Milling)
2.2.2
Control elements on the MCP
①
Reserved hole for emergency stop button
⑦
Axis traversing keys
②
Handwheel key
Controls the axis movement with external handwheels
⑧
Spindle override switch
(unavailable for the vertical MCP with a reserved slot
for the handwheel)
③
Tool number display
Displays the current tool number
⑨
Spindle state keys
④
Operating mode keys
⑩
Feedrate override switch
Traverses the selected axis at the specified feedrate
override
⑤
Program control keys
⑪
Keys for program start, stop, and reset
⑥
User-defined keys
⑫
Reserved slot for the handwheel

Programming and Operating Manual (Turning)
6FC5398-5DP10-0BA2, 06/2015 11
User-defined keys
Pressing this in any operating mode switches on/off the lamp.
LED on: The lamp is switched on.
LED off: The lamp is switched off.
Pressing this key in any operating mode switches on/off the coolant supply.
LED on: The coolant supply is switched on.
LED off: The coolant supply is switched off.
Pressing this key starts sequential tool changes (active only in "JOG" mode).
LED on: The machine starts sequential tool changes
LED off: The machine stops sequential tool changes
Pressing this key in any operating mode activates the chuck to clamp/unclamp the workpiece.
LED on: Activates the chuck to clamp the workpiece
LED off: Activates the chuck to unclamp the workpiece
Pressing this key only when the spindle stops operation.
LED on: Activates the external chuck to clamp the workpiece inwards
LED off: Activates the internal chuck to clamp the workpiece outwards
Pressing this key in any operating mode advances/retracts the tailstock.
LED on: Advances the tailstock towards the workpiece until it firmly engages with the end of the workpiece
Pre-defined insertion strips
The MCP package includes two sets (six pieces each) of pre-defined insertion strips. One set is for the turning variant of the
control system and is pre-inserted on the back of the MCP. The other set is for the milling variant of the control system.
If your control system is a milling variant of the control system, replace the pre-inserted strips with the milling-specific
insertion strips.

Programming and Operating Manual (Turning)
12 6FC5398-5DP10-0BA2, 06/2015
Customized insertion strips
The MCP package also includes an A4-sized blank plastic sheet with detachable strips. You can customize insertion strips if
the pre-defined strips cannot meet your needs.
In the \examples\SINUMERIK_808D_ADVANCED\MCP folder of the Toolbox DVD for the control system, there is a symbol
library file and an insertion strip template file. To make customized insertion strips, follow the steps below:
1. Copy the desired symbols from the symbol library file to the desired locations in the insertion strip template.
2. Print the template to the A4-sized blank plastic sheet.
3. Detach the insertion strips from the blank plastic sheet.
4. Pull out the pre-inserted strips from the MCP.
5. Insert the customized strips on the back of the MCP.
Note
This manual assumes a SINUMERIK 808D ADVANCED standard MCP. Should you use a different MCP, the operation
may be other than described herein.
2.3
Screen layout
Display of variable increments in the status area
Displays the variable increment if it is defined in the standard subroutine program
•Value ≤ five digits: displays the complete value
•Value > five digits: displays the first four digits plus ".."

Programming and Operating Manual (Turning)
6FC5398-5DP10-0BA2, 06/2015 13
Alarms and messages
Displays active alarms with alarm text
The alarm number is displayed in white lettering on a red back-
ground. 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 indicates the total number of active
alarms. When more than one alarm is active, the display scrolls
through the alarms in sequence. An acknowledgement symbol
indicates the alarm cancel criterion.
Displays messages from NC programs
Messages from NC programs do not have numbers and appear
in green lettering.
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

Programming and Operating Manual (Turning)
14 6FC5398-5DP10-0BA2, 06/2015
Protection level 7
Protection level 7 is set automatically if no password is set and no protection level interface signal is set. The protection level
7 can be set from the PLC user program by setting the bits in the user interface.
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 password
You can set the desired password through the following operating area:
+ →
2.5
Setting user interface language
Operating sequence
+
1. Select the desired operating area.
2. Press this softkey to 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.
Note:
The HMI (Human Machine Interface) is automatically restarted when a new language is
selected.

Programming and Operating Manual (Turning)
6FC5398-5DP10-0BA2, 06/2015 15
3
Turning on, reference point approach
Note
When turning on the CNC and the machine, also observe the machine tool manufacturer's documentation, since turning-on
and reference point approach are machine-dependent functions.
Operating sequence
1. Switch on the power supply for the control system and the machine.
2. Release all emergency stop buttons on the machine.
By default, the control system is in the "REF.POINT" window after booting.
The symbol shown next to the axis identifier indicates that the axis is not yet referenced.
If an axis is not reference
d, the symbol is always visible in the current (machining) operating
area.
3. Press the corresponding axis traversing keys on the MCP to traverse each axis to the refer-
ence point.
If the axis is referenced, a symbol ( ) appears next to the axis identifier and is visible only
in the "REF.POINT" window.
Note that axis traversing directions and axis key functions are defined by the machine man-
ufacturer.

Programming and Operating Manual (Turning)
16 6FC5398-5DP10-0BA2, 06/2015
4
Setting-up
4.1
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 so-called "3-finger rule" of the right hand. 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 "3-finger rule" of the right hand. 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.

Programming and Operating Manual (Turning)
6FC5398-5DP10-0BA2, 06/2015 17
The figure below shows an example of the machine coordinate system of a turning machine.
The origin of this coordinate system is the
machine zero.
This point is only a reference point which is defined by the machine manufacturer. It does not have to be approachable.
The traversing range of the
machine axes
can be in the negative range.
Workpiece coordinate system (WCS)
To describe the geometry of a workpiece in the workpiece program, a right-handed, right-angled coordinate system is also
used.
The
workpiece zero
can be freely selected by the programmer in the Z axis. In the X axis, it lies in the turning center.
The figure below shows an example of the workpiece coordinate system.
Relative coordinate system (REL)
In addition to the machine and workpiece coordinate systems, the control system provides a relative coordinate system. This
coordinate system is used to set reference points that can be freely selected and have no influence on the active workpiece
coordinate system. All axis movements are displayed relative to these reference points.
Clamping the workpiece
For machining, the workpiece is clamped on the machine. The workpiece must be aligned such that the axes of the
workpiece coordinate system run in parallel with those of the machine. Any resulting offset of the machine zero with
reference to the workpiece zero is determined along the Z axis and entered in a data area intended for the
settable work
offset
. In the NC program, this offset is activated during program execution, for example, using a programmed
G54
command.

Programming and Operating Manual (Turning)
18 6FC5398-5DP10-0BA2, 06/2015
The figure below shows an example of the workpiece clamped on the machine.
Current workpiece coordinate system
The programmed work offset TRANS (Page 56) can be used to generate an offset with reference to the workpiece
coordinate system, resulting in the current workpiece coordinate system.
4.2
Setting up tools
4.2.1
Creating a new tool
Note
The control system supports a maximum of 64 tools or 128 cutting edges.
Operating sequence
1. Select the desired operating area.
2. Open the tool list window.
3. Open the lower-level menu for tool type selection.
4. Select a desired tool type with the corresponding softkey.

Programming and Operating Manual (Turning)
6FC5398-5DP10-0BA2, 06/2015 19
5. Enter the tool number (value range: 1 to 31999; preferentially enter a value less than 100)
and select the corresponding tool edge position code according to the actual tool point di-
rection in the following windows:
•Available edge positions for turning tool and grooving tool: 1, 2, 3 and 4 (taking new
turning tool as an example)
•Available edge positions for drilling tool, tapping tool and milling tool: 5, 6, 7 and 8
(taking new milling tool as an example)
6. Use this softkey to confirm your settings. The window below shows the information of the
new tool created.
①Tool type
②Tool number
③Tool offset number
④Tool offset number
⑤Tool length in the X and Z axes
⑥Tool radius
⑦Clearance angle
⑧Tip width of the cutting edge, which is only active for the grooving tool
⑨Cutting edge direction

Programming and Operating Manual (Turning)
20 6FC5398-5DP10-0BA2, 06/2015
Note:
•Column ④is invisible in Siemens mode. The function of activating the compensation
data via the "H" column is active only in ISO dialect mode.
•Column ⑦is visible only when you set bit 18 of MD19730 to 1, that is, MD19730 =
40000H. By default, MD19730 = 0H. Note that MD19730 is visible only with the
manufacturer password. For more information about the clearance angle, see the
SINUMERIK 808D/SINUMERIK 808D ADVANCED Function Manual.
7. Enter the tool radius data or tool tip width as desired and confirm your settings.
4.2.2
Activating the tool
Operating sequence
1. Select the desired operating area.
2. Switch to "JOG" mode.
3. Open the "T, S, M" window.
4. Enter the desired tool number (for example, 1) in the "T, S, M" window.
5. Use this key or move the cursor to confirm your entries.
6. Press this key on the MCP to activate the tool.