Siemens SINUMERIK 808D User manual

© Siemens AG 2014. All rights reserved
6FC5398-4DP10-0BA1, 01/2014 1
SINUMERIK
SINUMERIK 808D ADVANCED
Programming and Operating Manual (Milling)
User Manual
Legal information
Warning notice system
This manual contains notices you have to observe in order to ensure your personal safety, as well as to prevent damage to property. The
notices referring to your personal safety are highlighted in the manual by a safety alert symbol, notices referring only to property damage
have no safety alert symbol. These notices shown below are graded according to the degree of danger.
DANGER
indicates that death or severe personal injury 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 (Milling)
26FC5398-4DP10-0BA1, 01/2014
Preface
Applicable products
This manual is applicable to the following control system:
Control system
Softvare version
SINUMERIK 808D ADVANCED M (Milling) V4.6
Documentation components and target groups
Component
Recommended target group
User documentation
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
Turning)
Programmers and operators of turning machines
Diagnostics Manual Mechanical and electrical designers, commissioning
engineers, machine operators, and service and
maintenance personnel
Manufacturer/service documentation
Commissioning Manual Installation personnel, commissioning engineers, and
service and maintenance personnel
Function Manual Mechanical and electrical designers, technical professionals
Parameter Manual Mechanical and electrical designers, technical professionals
PLC Subroutines Manual Mechanical and electrical designers, technical
professionals, and commissioning engineers
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
Hotline:
●Global support hotline:
[phone]
●Support hotline in China:
[phone] (china)
Service and Support:
●Chinese Web site:
http://www.siemens.com.cn/808D
●Global Web site:
http://support.automation.siemens.com
EC Declaration of Conformity
The EC Declaration of Conformity for the EMC Directive can be found on the Internet at
http://support.automation.siemens.com
Here, enter the number
15257461
as the search term or contact your local Siemens office.

Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA1, 01/2014 3
Table of contents
Preface...................................................................................................................................................................2
1 Introduction.............................................................................................................................................................7
1.1 SINUMERIK 808D ADVANCED operator panels..........................................................................................7
1.1.1 Overview.......................................................................................................................................................7
1.1.2 Control elements on the PPU........................................................................................................................8
1.2 Machine control panels ...............................................................................................................................10
1.2.1 Overview.....................................................................................................................................................10
1.2.2 Control elements on the MCP.....................................................................................................................11
1.3 Screen layout..............................................................................................................................................13
1.4 Protection levels..........................................................................................................................................14
1.5 Setting user interface language ..................................................................................................................15
2 Turning on, reference point approach ....................................................................................................................15
3 Setting-up.............................................................................................................................................................16
3.1 Coordinate systems ....................................................................................................................................16
3.2 Setting up tools ...........................................................................................................................................19
3.2.1 Creating a new tool .....................................................................................................................................19
3.2.2 Activating the tool........................................................................................................................................20
3.2.3 Assigning the handwheel ............................................................................................................................20
3.2.4 Activating the spindle..................................................................................................................................22
3.2.5 Measuring the tool (manually).....................................................................................................................23
3.2.6 Setting up the workpiece.............................................................................................................................25
3.2.7 Verifying the tool offset result in "MDA" mode.............................................................................................28
3.2.8 Entering/modifying the tool wear data.........................................................................................................29
3.3 Operating area overview.............................................................................................................................30
4 Part programming.................................................................................................................................................31
4.1 Creating a part program..............................................................................................................................32
4.2 Editing part programs..................................................................................................................................33
4.3 Managing part programs.............................................................................................................................35
5 Automatic machining.............................................................................................................................................37
5.1 Performing the simulation ...........................................................................................................................38
5.2 Program control ..........................................................................................................................................39
5.3 Program test ...............................................................................................................................................41
5.4 Starting and stopping / interrupting a part program.....................................................................................42
5.5 Executing / transferring a part program through the RS232 interface .........................................................43
5.5.1 Configuring RS232 communication.............................................................................................................43
5.5.2 Executing from external (through RS232 interface) ....................................................................................44
5.5.3 Transferring from external (through RS232 interface).................................................................................45
5.6 Machining at a specific point.......................................................................................................................46
6 Saving system data...............................................................................................................................................47
7 Data backup .........................................................................................................................................................49
8 Programming principles ........................................................................................................................................50
8.1 Fundamentals of programming ...................................................................................................................50
8.1.1 Program names ..........................................................................................................................................50
8.1.2 Program structure .......................................................................................................................................50
8.2 Positional data ............................................................................................................................................51

Programming and Operating Manual (Milling)
46FC5398-4DP10-0BA1, 01/2014
8.2.1 Programming dimensions........................................................................................................................... 51
8.2.2 Plane selection: G17 to G19....................................................................................................................... 51
8.2.3 Absolute/incremental dimensioning: G90, G91, AC, IC .............................................................................. 52
8.2.4 Dimensions in metric units and inches: G71, G70, G710, G700................................................................. 53
8.2.5 Polar coordinates, pole definition: G110, G111, G112................................................................................ 54
8.2.6 Programmable work offset: TRANS, ATRANS ........................................................................................... 56
8.2.7 Programmable rotation: ROT, AROT.......................................................................................................... 56
8.2.8 Programmable scaling factor: SCALE, ASCALE ........................................................................................ 58
8.2.9 Programmable mirroring: MIRROR, AMIRROR.......................................................................................... 58
8.2.10 Workpiece clamping - settable work offset: G54 to G59, G500, G53, G153............................................... 60
8.2.11 NC block compression (COMPON, COMPCURV, COMPCAD) ................................................................. 61
8.2.12 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......................................................................................................... 70
8.4 Circular interpolation................................................................................................................................... 72
8.4.1 Circular interpolation: G2, G3 ..................................................................................................................... 72
8.4.2 Circular interpolation via intermediate point: CIP........................................................................................ 76
8.4.3 Circle with tangential transition: CT ............................................................................................................ 77
8.4.4 Helix interpolation: G2/G3, TURN............................................................................................................... 78
8.4.5 Feedrate override for circles: CFTCP, CFC................................................................................................ 78
8.5 Thread cutting............................................................................................................................................. 79
8.5.1 Thread cutting with constant lead: G33 ...................................................................................................... 79
8.5.2 Tapping with compensating chuck: G63..................................................................................................... 80
8.5.3 Thread interpolation: G331, G332 .............................................................................................................. 81
8.6 Fixed point approach .................................................................................................................................. 82
8.6.1 Fixed point approach: G75 ......................................................................................................................... 82
8.6.2 Reference point approach: G74.................................................................................................................. 83
8.7 Acceleration control and exact stop/continuous path.................................................................................. 84
8.7.1 Acceleration pattern: BRISK, SOFT............................................................................................................ 84
8.7.2 Exact stop/continuous-path control mode: G9, G60, G64........................................................................... 84
8.7.3 Dwell time: G4 ............................................................................................................................................ 86
8.8 Spindle movements .................................................................................................................................... 87
8.8.1 Gear stages................................................................................................................................................ 87
8.8.2 Spindle speed S, directions of rotation ....................................................................................................... 87
8.8.3 Spindle positioning: SPOS.......................................................................................................................... 88
8.9 Contour programming support.................................................................................................................... 88
8.9.1 Contour definition programming ................................................................................................................. 88
8.9.2 Rounding, chamfer ..................................................................................................................................... 90
8.10 Tool and tool offset..................................................................................................................................... 93
8.10.1 General Information.................................................................................................................................... 93
8.10.2 Tool T ......................................................................................................................................................... 94
8.10.3 Tool compensation number D..................................................................................................................... 94
8.10.4 Selecting the tool radius compensation: G41, G42..................................................................................... 96
8.10.5 Corner behavior: G450, G451 .................................................................................................................... 99
8.10.6 Tool radius compensation OFF: G40........................................................................................................ 100
8.10.7 Special cases of the tool radius compensation......................................................................................... 101
8.10.8 Example of tool radius compensation....................................................................................................... 102
8.11 Miscellaneous function M ......................................................................................................................... 103
8.12 H function ................................................................................................................................................. 103
8.13 Arithmetic parameters, LUD and PLC variables ....................................................................................... 104
8.13.1 Arithmetic parameter R............................................................................................................................. 104
8.13.2 Local User Data (LUD) ............................................................................................................................. 105
8.13.3 Reading and writing PLC variables........................................................................................................... 106
8.14 Program jumps ......................................................................................................................................... 107
8.14.1 Unconditional program jumps................................................................................................................... 107
8.14.2 Conditional program jumps....................................................................................................................... 108
8.14.3 Program example for jumps...................................................................................................................... 109

Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA1, 01/2014 5
8.14.4 Jump destination for program jumps.........................................................................................................110
8.15 Subroutine technique ................................................................................................................................110
8.15.1 General information...................................................................................................................................110
8.15.2 Calling machining cycles...........................................................................................................................112
8.15.3 Modal subroutine call ................................................................................................................................113
8.15.4 Execute external subroutine (EXTCALL) ..................................................................................................113
8.16 Timers and workpiece counters ................................................................................................................114
8.16.1 Runtime timer............................................................................................................................................114
8.16.2 Workpiece counter ....................................................................................................................................116
8.17 Smooth approach and retraction...............................................................................................................117
9 Cycles ................................................................................................................................................................ 121
9.1 Overview of cycles ....................................................................................................................................121
9.2 Programming cycles..................................................................................................................................122
9.3 Graphical cycle support in the program editor...........................................................................................124
9.4 Drilling cycles ............................................................................................................................................125
9.4.1 General information...................................................................................................................................125
9.4.2 Requirements............................................................................................................................................125
9.4.3 Drilling, centering - CYCLE81 ...................................................................................................................126
9.4.4 Drilling, counterboring - CYCLE82 ............................................................................................................128
9.4.5 Deep-hole drilling - CYCLE83 ...................................................................................................................130
9.4.6 Rigid tapping - CYCLE84 ..........................................................................................................................135
9.4.7 Tapping with compensating chuck - CYCLE840.......................................................................................139
9.4.8 Reaming 1 - CYCLE85..............................................................................................................................144
9.4.9 Boring - CYCLE86.....................................................................................................................................145
9.4.10 Boring with stop 1 - CYCLE87 ..................................................................................................................148
9.4.11 Drilling with stop 2 - CYCLE88..................................................................................................................150
9.4.12 Reaming 2 - CYCLE89..............................................................................................................................151
9.5 Drilling pattern cycles ................................................................................................................................153
9.5.1 Requirements............................................................................................................................................153
9.5.2 Row of holes - HOLES1............................................................................................................................154
9.5.3 Circle of holes - HOLES2..........................................................................................................................157
9.5.4 Arbitrary positions - CYCLE802 ................................................................................................................160
9.6 Milling cycles.............................................................................................................................................161
9.6.1 Requirements............................................................................................................................................161
9.6.2 Face milling - CYCLE71............................................................................................................................162
9.6.3 Contour milling - CYCLE72 .......................................................................................................................167
9.6.4 Milling a rectangular spigot - CYCLE76 ....................................................................................................177
9.6.5 Milling a circular spigot -CYCLE77...........................................................................................................181
9.6.6 Long holes located on a circle - LONGHOLE............................................................................................184
9.6.7 Slots on a circle - SLOT1 ..........................................................................................................................187
9.6.8 Circumferential slot - SLOT2.....................................................................................................................192
9.6.9 Milling a rectangular pocket - POCKET3...................................................................................................197
9.6.10 Milling a circular pocket - POCKET4.........................................................................................................203
9.6.11 Thread milling - CYCLE90 ........................................................................................................................206
9.6.12 High speed settings - CYCLE832..............................................................................................................210
9.7 Error messages and error handling...........................................................................................................211
9.7.1 General Information ..................................................................................................................................211
9.7.2 Error handling in the cycles.......................................................................................................................211
9.7.3 Overview of cycle alarms ..........................................................................................................................211
9.7.4 Messages in the cycles.............................................................................................................................211
10 Typical milling program ....................................................................................................................................... 212
A Appendix ............................................................................................................................................................ 218
A.1 Creating a new cutting edge .....................................................................................................................218
A.2 Calibrating the tool probe..........................................................................................................................219
A.3 Measuring the tool with a probe (auto)......................................................................................................220
A.4 Entering/modifying work offsets ................................................................................................................222

Programming and Operating Manual (Milling)
66FC5398-4DP10-0BA1, 01/2014
A.5 Entering/modifying the setting data........................................................................................................... 222
A.6 Setting R parameters................................................................................................................................ 225
A.7 Setting user data....................................................................................................................................... 225
A.8 Other settings in "JOG" mode................................................................................................................... 226
A.8.1 Setting the relative coordinate system (REL)............................................................................................ 227
A.8.2 Face milling .............................................................................................................................................. 228
A.8.3 Setting the JOG data ................................................................................................................................ 229
A.9 The help system ....................................................................................................................................... 230
A.10 Operation wizard....................................................................................................................................... 232
A.11 Editing Chinese characters....................................................................................................................... 232
A.12 Pocket calculator ...................................................................................................................................... 233
A.13 Calculating contour elements ................................................................................................................... 234
A.14 Free contour programming ....................................................................................................................... 238
A.14.1 Programming a contour ............................................................................................................................ 239
A.14.2 Defining a start point................................................................................................................................. 240
A.14.3 Programming contour element ................................................................................................................. 241
A.14.4 Parameters for contour elements.............................................................................................................. 243
A.14.5 Specifying contour elements in polar coordinates..................................................................................... 246
A.14.6 Cycle support............................................................................................................................................ 248
A.14.7 Programming example for milling ............................................................................................................. 248
A.15 Word structure and address ..................................................................................................................... 256
A.16 Character set ............................................................................................................................................ 257
A.17 Block format.............................................................................................................................................. 257
A.18 List of instructions..................................................................................................................................... 258

Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA1, 01/2014 7
1
Introduction
1.1
SINUMERIK 808D ADVANCED operator panels
1.1.1
Overview
The SINUMERIK 808D ADVANCED PPU (Panel Processing Unit) is available in the following variants:
●PPU161.2
horizontal panel layout, applicable for the SINUMERIK 808D ADVANCED T (turning) or SINUMERIK 808D ADVANCED
M (milling) control system
●PPU160.2
vertical panel layout, applicable for the SINUMERIK 808D ADVANCED T (turning) or SINUMERIK 808D ADVANCED M
(milling) control system
PPU161.2 (horizontal panel layout)
PPU160.2 (vertical panel layout)

Programming and Operating Manual (Milling)
86FC5398-4DP10-0BA1, 01/2014
1.1.2
Control elements on the PPU
Elements on the PPU (Panel Processing Unit) front
The following illustration uses PPU161.2 as an example to show control elements available on the PPU:
①
Vertical and horizontal softkeys
Calls specific menu functions
⑦
On-board wizard key
Provides step-by-step guides on basic commissioning
and operation procedures
②
Return key
Returns to the next higher-level menu
⑧
Help key
Calls help information
③
Menu extension key
Opens the next lower-level menu or navigate between
the menus of the same level
⑨
Cursor keys
*
④
Alphabetic and numeric keys
* ⑩
Operating area keys
*
⑤
Control keys
* ⑪
USB interface
*
⑥
Alarm cancellation key
Cancels alarms and messages that are marked with
this symbol
⑫
Status LEDs
*
* For more information, refer to the table below.
Further information
Alphabetic and
numeric keys
To enter the upper character on an alphabetic/numeric key, keep the following key
pressed:
The icons on the following keys are available only with PPU161.2 and PPU160.2.
The icon on the key is a hint that you can press both <CTRL> and this key as
shortcuts for capturing screens.

Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA1, 01/2014 9
The icon on the key is a hint that you can press both <CTRL> and this key as
shortcuts for saving start-up archives.
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.
The icon on the key is a hint that you can press this key to call the calculator function.
Cursor keys
●Toggles between entries in the input field
●Enters the "Set-up menu" dialog at NC start-up
Icons on both keys are available only with PPU161.2 and PPU160.2. The icon on the
key is a hint that you can press both <CTRL> and the key to adjust the screen
backlight brightness.
Control keys The icon on the key is available only with PPU161.2 and PPU160.2. The icon is a hint
that this key can be used together with another key to function as a key combination.
Operating area
keys
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, refer to SINUMERIK 808D ADVANCED
Function Manual.
Status LEDs LED "POK"
Lights up green: The power supply for the CNC is switched on.
LED "RDY"
Lights up green: The CNC is ready and the PLC is in running mode.
Lights up orange:
●On: The PLC is in stop mode.
●Flashing: The PLC is in power-up mode.
Lights up red: The CNC is in stop mode.
LED "TEMP"
Unlit: The CNC temperature is within the specified range.
Lights up orange: The CNC temperature is out of range.
USB interface Connects to a USB device, for example:
●An external USB memory sticker, to transfer data between the USB sticker and the
CNC
●
An external USB keyboard which functions as an external NC keyboard

Programming and Operating Manual (Milling)
10 6FC5398-4DP10-0BA1, 01/2014
1.2
Machine control panels
1.2.1
Overview
Elements on the MCP (Machine Control Panel) front
The SINUMERIK 808D MCP is available in the following variants:
●Horizontal MCP variant
●Vertical MCP variant with a reserved slot for the handwheel
●Vertical MCP variant with an override switch for the spindle
Horizontal MCP
Vertical MCP with reserved handwheel slot Vertical MCP with spindle override switch

Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA1, 01/2014 11
1.2.2
Control elements on the MCP
Elements on the MCP (Machine Control Panel) front
The following illustration uses a horizontal MCP as an example to show control elements available 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 reserved
handwheel slot)
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
*
* For more information, refer to the table below.
Further information
User-defined keys Pressing this in any operating mode switches on/off the lamp.
LED lit: The lamp is switched on.
LED unlit: The lamp is switched off.
Pressing this key in any operating mode switches on/off the coolant
supply.
LED lit: The coolant supply is switched on.
LED unlit: The coolant supply is switched off.
When all axes and the spindle stop operation, pressing this key unlocks
the safety door.
LED lit: The safety door is unlocked.
LED unlit: The safety door is locked.
Pressing this key rotates the magazine clockwise (active only in JOG
mode).
LED lit: The magazine rotates clockwise.
LED unlit: The magazine stops clockwise rotation.

Programming and Operating Manual (Milling)
12 6FC5398-4DP10-0BA1, 01/2014
Pressing this key approaches the magazine to the reference point
(active only in JOG mode).
LED on: The magazine is reference point approached.
LED off: The magazine is not yet referenced
Pressing this key rotates the magazine counter-clockwise (active only in
JOG mode).
LED on: The magazine rotates counter-clockwise.
LED off: The magazine stops counter-clockwise rotation.
Pressing this key in any operating mode starts the forward rotation of the
chip remover (active only in JOG mode).
LED lit: The chip remover starts forward rotation.
LED unlit: The chip remover stops rotation.
Keeping pressing this key in any operating mode rotates the chip
remover in reverse order. Releasing the key changes the chip remover
to the previous forward rotation or stop state (active only in JOG mode).
LED lit: The chip remover starts reverse rotation.
LED unlit: The chip remover stops reverse rotation.
Pre-defined insertion strips
The MCP (machine control panel) 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 of the SINUMERIK 808D ADVANCED milling variant, replace the pre-inserted strips with the milling-
specific insertion strips.

Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA1, 01/2014 13
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 can not meet your needs.
In the \examples\MCP folder of the Toolbox DVD for the SINUMERIK 808D ADVANCED, 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 an 808D standard machine control panel (MCP). Should you use a different MCP, the operation
may be other than described herein.
1.3
Screen layout
Alarms and messages
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
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.

Programming and Operating Manual (Milling)
14 6FC5398-4DP10-0BA1, 01/2014
1.4
Protection levels
Overview
The SINUMERIK 808D ADVANCED 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 and drive data
●Editing programs
●Setting offset values
●Measuring tools
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
●RS232 settings
●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:
+ →

Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA1, 01/2014 15
1.5
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.
2
Turning on, reference point approach
Note
When turning on/off 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 on the screen indicates that the axis is not yet referenced. If an axis is not
referenced, the symbol is always visible in the current (machining) operating area.

Programming and Operating Manual (Milling)
16 6FC5398-4DP10-0BA1, 01/2014
3. Press the corresponding axis traversing keys to traverse each axis to the reference point.
If an axis is referenced, a symbol ( ) is shown 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
manufacturer.
3
Setting-up
3.1
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.

Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA1, 01/2014 17
Machine coordinate system (MCS)
The orientation of the coordinate system relative to the machine depends on the respective machine types. 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.
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.
The figure below shows an example of the workpiece coordinate system.

Programming and Operating Manual (Milling)
18 6FC5398-4DP10-0BA1, 01/2014
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 references.
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 X, Y and 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.
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.

Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA1, 01/2014 19
3.2
Setting up tools
3.2.1
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.
5. Enter the tool number (value range: 1 to 31999; preferentially enter a value less than 100) in the
following window.
Note:
Select the corresponding tool edge position code according to the actual tool point direction.
6. Use this softkey to confirm your settings. The window below shows the information of the new tool
created.
①Tool type ③Cutting edge number
②Tool number ④Tool length and radius

Programming and Operating Manual (Milling)
20 6FC5398-4DP10-0BA1, 01/2014
7. Enter the tool radius data and confirm your settings.
3.2.2
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.
3.2.3
Assigning the handwheel
Method 1: Assigning through the MCP
1. Select the desired operating area.
2. Press this key on the MCP to control the axis movement with external handwheels.
3. Press the desired axis traversing key with the handwheel icon. The handwheel is assigned.