Siemens SINUMERIK 808D Operation & User’s Manual
Read Online
Read the Siemens SINUMERIK 808D Operation & User’s Manual online using the built-in PDF viewer.
Text of the manual
© Siemens AG 2017. All rights reserved
6FC5398-4DP10-0BA6, 09/2017
1
SINUMERIK
SINUMERIK 808D, SINUMERIK 808D ADVANCED
Programming and Operating Manual (Milling)
User Manual
Legal information
Warning notice system
This manual contains notices you have to observe in order to ensure your personal safety, as well as to prevent damage to property. The
notices referring to your personal safety are highlighted in the manual by a safety alert symbol, notices referring only to property damage
have no safety alert symbol. These notices shown below are graded according to the degree of danger.
DANGER
indicates that death or severe personal injury 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)
2
6FC5398-4DP10-0BA6, 09/2017
Preface
Applicable products
This manual is valid for the following control systems:
Control system
Software version
SINUMERIK 808D ADVANCED M (Milling)
V4.8.1.2: PPU16x.3/PPU15x.3 with spindle/feed servo system
SINUMERIK 808D (Milling)
V4.8.1.1: PPU141.3 with feed servo system
Documentation components and target audience
End-user documentation
Target audience
Programming and Operating Manual (Turning)
Programmers and operators of turning machines
Programming and Operating Manual (Milling)
Programmers and operators of milling machines
Programming and Operating Manual (ISO Turning/Milling) Programmers and operators of turning/milling machines
Programming and Operating Manual (Manual Machine
Plus (MM+), Turning)
Programmers and operators of turning machines
Diagnostics Manual
Mechanical and electrical designers, commissioning engi-
neers, machine operators, and service and maintenance per-
sonnel
Manufacturer/service documentation
Target audience
Commissioning Manual
Installation personnel, commissioning engineers, and service
and maintenance personnel
Function Manual
Mechanical and electrical designers, technical professionals
Parameter Manual
Mechanical and electrical designers, technical professionals
Service Manual
Mechanical and electrical designers, technical professionals,
commissioning engineers, and service and maintenance per-
sonnel
Readme file
Third-party software - Licensing terms and copyright information
My Documentation Manager (MDM)
Under the following link you will find information to individually compile your documentation based on the Siemens content:
www.siemens.com/mdm
Standard scope
This manual only describes the functionality of the standard version. Extensions or changes made by the machine tool
manufacturer are documented by the machine tool manufacturer.
Technical support
Country
Hotline 1)
Further service contact information:
•
Worldwide Web site:
https://support.industry.siemens.com/cs/ww/en/
•
Chinese Web site:
http://www.siemens.com.cn/808D
Germany
+49 911 895 7222
China
+86 400 810 4288
1) You can find more hotline information at the worldwide Web site given above.
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
3
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 (Milling)
4
6FC5398-4DP10-0BA6, 09/2017
Table of contents
Preface............................................................................................................................................... 2
1
Fundamental safety instructions .............................................................................................................. 8
1.1
General safety instructions.....................................................................................................................................8
1.2
Warranty and liability for application examples...................................................................................................8
1.3
Industrial security .....................................................................................................................................................9
2
Introduction ......................................................................................................................................... 9
2.1
Panel Processing Units (PPUs).............................................................................................................................9
2.1.1
PPU versions............................................................................................................................................................9
2.1.2
PPU control elements .......................................................................................................................................... 10
2.1.3
Screen layout......................................................................................................................................................... 12
2.2
Machine Control Panels (MCPs) ........................................................................................................................ 13
2.2.1
MCP versions ........................................................................................................................................................ 13
2.2.2
MCP control elements.......................................................................................................................................... 13
2.3
Coordinate systems.............................................................................................................................................. 16
2.4
Protection levels.................................................................................................................................................... 18
3
Common notices for machining operations............................................................................................... 20
4
Switching on and referencing ................................................................................................................ 20
5
Setting the user interface language ........................................................................................................ 21
6
Setting up tools .................................................................................................................................. 21
6.1
Creating a tool ....................................................................................................................................................... 21
6.2
Creating/changing a cutting edge ...................................................................................................................... 22
6.3
Activating the tool and the spindle ..................................................................................................................... 23
6.4
Assigning the handwheel..................................................................................................................................... 24
6.4.1
Assigning the handwheel through the MCP ..................................................................................................... 24
6.4.2
Assigning the handwheel through the PPU...................................................................................................... 25
6.5
Measuring the tool manually ............................................................................................................................... 27
6.6
Verifying the tool offset result ............................................................................................................................. 28
7
Creating part programs ........................................................................................................................ 29
7.1
Creating a part program....................................................................................................................................... 29
7.2
Editing the part program ...................................................................................................................................... 31
7.2.1
Using a standard program structure .................................................................................................................. 31
7.2.2
Editing a part program ......................................................................................................................................... 31
7.2.3
Understanding frequently used programming instructions ............................................................................ 37
7.2.3.1
Inch or metric dimensions (G70/G71) ............................................................................................................... 37
7.2.3.2
Definition of work offset (G54 to G59, G500, G90/G91) ................................................................................ 37
7.2.3.3
Rapid traverse (G00)............................................................................................................................................ 38
7.2.3.4
Tool and traverse (T, D, M6, F, G94/G95, S, M3/M4, G01) .......................................................................... 39
7.2.3.5
Tool radius compensation (G40, G41/G42) ..................................................................................................... 39
7.2.3.6
Milling circles and arcs (G02/G03)..................................................................................................................... 40
7.2.3.7
Fixed point approach (G74/G75)........................................................................................................................ 41
7.2.3.8
Spindle control....................................................................................................................................................... 42
7.2.3.9
Setting dwell time in the program (G04) ........................................................................................................... 42
8
Program simulation ............................................................................................................................. 42
8.1
Simulation prior to machining of the workpiece ............................................................................................... 43
8.2
Simultaneous recording prior to machining of the workpiece........................................................................ 45
9
Machining the workpiece ...................................................................................................................... 46
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
5
9.1
Executing a part program.....................................................................................................................................46
9.2
Executing specified blocks...................................................................................................................................47
9.3
Correcting a part program ....................................................................................................................................48
9.4
Simultaneous recording during machining of the workpiece..........................................................................48
9.5
Entering the tool wear offsets ..............................................................................................................................49
10
Other common operations .................................................................................................................... 53
10.1
Program control functions ....................................................................................................................................53
10.1.1
Program test...........................................................................................................................................................53
10.1.2
Dry run feedrate.....................................................................................................................................................53
10.1.3
Conditional stop .....................................................................................................................................................53
10.1.4
Skip block ...............................................................................................................................................................53
10.1.5
Single block mode .................................................................................................................................................53
10.1.6
Rapid traverse override ........................................................................................................................................54
10.1.7
Auxiliary function lock ...........................................................................................................................................54
10.2
Calibrating the tool probe .....................................................................................................................................54
10.3
Measuring the tool with a probe (auto) ..............................................................................................................56
10.4
Setting up the workpiece ......................................................................................................................................57
10.4.1
Measuring the workpiece .....................................................................................................................................57
10.4.2
Entering/modifying workpiece offsets ................................................................................................................59
10.5
Entering/modifying the setting data ....................................................................................................................60
10.6
Setting R parameters ............................................................................................................................................63
10.7
Setting user data ...................................................................................................................................................64
10.8
Setting the date and time .....................................................................................................................................64
10.9
Configuring the operating area after startup .....................................................................................................65
10.10
Executing/transferring a part program from external .......................................................................................65
10.10.1
Executing/transferring through the USB interface............................................................................................65
10.10.1.1
Executing from external (through USB interface) ............................................................................................66
10.10.1.2
Transferring from external (through USB interface) ........................................................................................67
10.10.2
Executing/transferring through the Ethernet connection.................................................................................67
10.10.2.1
Configuring the network drive..............................................................................................................................67
10.10.2.2
Executing from external (through Ethernet connection)..................................................................................70
10.10.2.3
Transferring from external (through Ethernet connection)..............................................................................70
10.10.3
Configuring the firewall .........................................................................................................................................71
10.11
Extending/deactivating the CNC lock function..................................................................................................72
10.12
Data backup ...........................................................................................................................................................74
10.12.1
Internal data backup .............................................................................................................................................74
10.12.2
External data backup ............................................................................................................................................75
10.12.2.1
External data backup in a data archive..............................................................................................................75
10.12.2.2
External data backup of separate files...............................................................................................................76
10.13
Pocket calculator ...................................................................................................................................................77
11
Programming principles........................................................................................................................ 78
11.1
Fundamentals of programming ...........................................................................................................................78
11.1.1
Program names .....................................................................................................................................................78
11.1.2
Program structure..................................................................................................................................................79
11.2
Programming instructions ....................................................................................................................................79
11.2.1
Programming dimensions ....................................................................................................................................79
11.2.2
Plane selection: G17 to G19................................................................................................................................80
11.2.3
Absolute/incremental dimensioning: G90, G91, AC, IC ..................................................................................81
11.2.4
Dimensions in metric units and inches: G71, G70, G710, G700 ...................................................................82
11.2.5
Polar coordinates, pole definition: G110, G111, G112....................................................................................82
11.2.6
Programmable work offset: TRANS, ATRANS.................................................................................................84
11.2.7
Programmable rotation: ROT, AROT .................................................................................................................85
11.2.8
Programmable scale factor: SCALE, ASCALE ................................................................................................86
11.2.9
Programmable mirroring: MIRROR, AMIRROR ...............................................................................................87
11.2.10
Workpiece coordinate system - settable work offset: G54 to G59, G500, G53, G153 ..............................88
Programming and Operating Manual (Milling)
6
6FC5398-4DP10-0BA6, 09/2017
11.2.11
NC block compression (COMPON, COMPCURV, COMPCAD) ................................................................... 89
11.3
Linear interpolation ............................................................................................................................................... 91
11.3.1
Linear interpolation with rapid traverse: G0...................................................................................................... 91
11.3.2
Feedrate F ............................................................................................................................................................. 92
11.3.3
Linear interpolation with feedrate: G1 ............................................................................................................... 92
11.4
Circular interpolation ............................................................................................................................................ 93
11.4.1
Circular interpolation: G2, G3 ............................................................................................................................. 93
11.4.2
Circular interpolation via intermediate point: CIP ............................................................................................ 98
11.4.3
Circle with tangential transition: CT ................................................................................................................... 99
11.4.4
Helix interpolation: G2/G3, TURN ...................................................................................................................... 99
11.4.5
Feedrate override for circles: CFTCP, CFC ................................................................................................... 100
11.5
Thread cutting ..................................................................................................................................................... 101
11.5.1
Thread cutting with constant lead: G33 .......................................................................................................... 101
11.5.2
Tapping with compensating chuck: G63 ......................................................................................................... 102
11.5.3
Thread interpolation: G331, G332 ................................................................................................................... 103
11.6
Fixed point approach.......................................................................................................................................... 104
11.6.1
Fixed point approach: G75 ................................................................................................................................ 104
11.6.2
Reference point approach: G74 ....................................................................................................................... 105
11.7
Acceleration control and exact stop/continuous path ................................................................................... 105
11.7.1
Acceleration pattern: BRISK, SOFT ................................................................................................................ 105
11.7.2
Exact stop/continuous-path control mode: G9, G60, G64 ........................................................................... 106
11.7.3
Dwell time: G4 ..................................................................................................................................................... 108
11.8
Spindle movements ............................................................................................................................................ 109
11.8.1
Gear stages ......................................................................................................................................................... 109
11.8.2
Spindle speed S, directions of rotation............................................................................................................ 109
11.8.3
Spindle positioning: SPOS ................................................................................................................................ 110
11.9
Contour programming support.......................................................................................................................... 110
11.9.1
Contour definition programming ....................................................................................................................... 110
11.9.2
Rounding, chamfer ............................................................................................................................................. 112
11.10
Tool and tool offset ............................................................................................................................................. 115
11.10.1
General Information............................................................................................................................................ 115
11.10.2
Tool T.................................................................................................................................................................... 116
11.10.3
Tool compensation number D........................................................................................................................... 116
11.10.4
Selecting the tool radius compensation: G41, G42....................................................................................... 119
11.10.5
Corner behavior: G450, G451 .......................................................................................................................... 121
11.10.6
Tool radius compensation OFF: G40 .............................................................................................................. 122
11.10.7
Special cases of the tool radius compensation.............................................................................................. 123
11.10.8
Example of tool radius compensation ............................................................................................................. 124
11.11
Miscellaneous function M .................................................................................................................................. 125
11.12
H function ............................................................................................................................................................. 125
11.13
Arithmetic parameters, LUD and PLC variables............................................................................................ 126
11.13.1
Arithmetic parameter R ...................................................................................................................................... 126
11.13.2
Local User Data (LUD)....................................................................................................................................... 127
11.13.3
Reading and writing PLC variables.................................................................................................................. 128
11.14
Program jumps .................................................................................................................................................... 129
11.14.1
Unconditional program jumps ........................................................................................................................... 129
11.14.2
Conditional program jumps ............................................................................................................................... 129
11.14.3
Program example for jumps .............................................................................................................................. 131
11.14.4
Jump destination for program jumps ............................................................................................................... 132
11.15
Subroutine technique ......................................................................................................................................... 132
11.15.1
General information ............................................................................................................................................ 132
11.15.2
Calling machining cycles ................................................................................................................................... 134
11.15.3
Modal subroutine call ......................................................................................................................................... 134
11.15.4
Executing internal and external subroutines (CALL, EXTCALL) ................................................................ 135
11.16
Timers and workpiece counters ....................................................................................................................... 136
11.16.1
Runtime timer ...................................................................................................................................................... 136
11.16.2
Workpiece counter.............................................................................................................................................. 138
11.17
Smooth approach and retraction...................................................................................................................... 139
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
7
11.18
Cylinder surface transformation (TRACYL) ................................................................................................... 144
11.19
Coupled motion (TRAILON, TRAILOF) .......................................................................................................... 150
12
Cycles ............................................................................................................................................ 152
12.1
Overview of cycles ............................................................................................................................................. 152
12.2
Programming cycles .......................................................................................................................................... 153
12.3
Graphical cycle programming in the program editor..................................................................................... 154
12.4
Drilling cycles ...................................................................................................................................................... 155
12.4.1
General information............................................................................................................................................ 155
12.4.2
Requirements...................................................................................................................................................... 156
12.4.3
Drilling, centering - CYCLE81 .......................................................................................................................... 157
12.4.4
Drilling, counterboring - CYCLE82 .................................................................................................................. 159
12.4.5
Deep-hole drilling - CYCLE83 .......................................................................................................................... 161
12.4.6
Rigid tapping - CYCLE84 .................................................................................................................................. 166
12.4.7
Tapping with compensating chuck - CYCLE840........................................................................................... 170
12.4.8
Reaming 1 - CYCLE85 ...................................................................................................................................... 175
12.4.9
Boring - CYCLE86.............................................................................................................................................. 176
12.5
Drilling pattern cycles......................................................................................................................................... 179
12.5.1
Requirements...................................................................................................................................................... 179
12.5.2
Row of holes - HOLES1 .................................................................................................................................... 179
12.5.3
Circle of holes - HOLES2 .................................................................................................................................. 182
12.5.4
Arbitrary positions - CYCLE802 ....................................................................................................................... 185
12.6
Milling cycles ....................................................................................................................................................... 186
12.6.1
Requirements...................................................................................................................................................... 186
12.6.2
Face milling - CYCLE71 .................................................................................................................................... 187
12.6.3
Contour milling - CYCLE72............................................................................................................................... 192
12.6.4
Milling a rectangular spigot - CYCLE76.......................................................................................................... 200
12.6.5
Milling a circular spigot - CYCLE77 ................................................................................................................. 204
12.6.6
Long holes located on a circle - LONGHOLE ................................................................................................ 207
12.6.7
Slots on a circle - SLOT1 .................................................................................................................................. 211
12.6.8
Circumferential slot - SLOT2 ............................................................................................................................ 216
12.6.9
Milling a rectangular pocket - POCKET3........................................................................................................ 221
12.6.10
Milling a circular pocket - POCKET4 ............................................................................................................... 226
12.6.11
Thread milling - CYCLE90 ................................................................................................................................ 230
12.6.12
High speed settings - CYCLE832 .................................................................................................................... 234
12.7
Error messages and error handling................................................................................................................. 234
12.7.1
General Information ........................................................................................................................................... 234
12.7.2
Error handling in the cycles .............................................................................................................................. 234
12.7.3
Overview of cycle alarms .................................................................................................................................. 235
12.7.4
Messages in the cycles ..................................................................................................................................... 235
13
Machining typical milling parts ............................................................................................................. 235
13.1
Operations before programming ...................................................................................................................... 235
13.2
Programming (Example 1) ................................................................................................................................ 236
13.3
Programming (Example 2) ................................................................................................................................ 245
13.4
Programming (Example 3) ................................................................................................................................ 252
13.5
Programming (Example 4) ................................................................................................................................ 267
13.6
Program simulation and execution .................................................................................................................. 278
A
Appendix......................................................................................................................................... 279
A.1
Operating area overview ................................................................................................................................... 279
A.1.1
Machining operating area.................................................................................................................................. 279
A.1.2
Program editing operating area ....................................................................................................................... 279
A.1.3
Offset operating area ......................................................................................................................................... 280
A.1.4
Program management operating area ............................................................................................................ 281
A.1.5
System data operating area.............................................................................................................................. 284
A.1.6
Alarm operating area ......................................................................................................................................... 286
A.2
Operating mode overview ................................................................................................................................. 287
A.2.1
"JOG" mode ........................................................................................................................................................ 287
Programming and Operating Manual (Milling)
8
6FC5398-4DP10-0BA6, 09/2017
A.2.1.1
Running the spindle manually .......................................................................................................................... 288
A.2.1.2
Executing M functions ........................................................................................................................................ 289
A.2.1.3
Setting the relative coordinate system (REL)................................................................................................. 290
A.2.1.4
Face milling.......................................................................................................................................................... 291
A.2.1.5
Setting the JOG data.......................................................................................................................................... 293
A.2.2
"AUTO" mode ...................................................................................................................................................... 294
A.2.3
"MDA" mode ........................................................................................................................................................ 295
A.3
Activating the contour handwheel via the NC program ................................................................................ 296
A.4
The help system.................................................................................................................................................. 298
A.5
Operation wizard................................................................................................................................................. 300
A.6
Editing Chinese characters ............................................................................................................................... 301
A.7
Calculating contour elements ........................................................................................................................... 302
A.8
Free contour programming................................................................................................................................ 306
A.8.1
Defining a start point .......................................................................................................................................... 307
A.8.2
Programming contour element ......................................................................................................................... 308
A.8.3
Parameters for contour elements..................................................................................................................... 311
A.8.4
Specifying contour elements in polar coordinates......................................................................................... 314
A.8.5
Cycle support....................................................................................................................................................... 316
A.8.6
Programming example for milling application ................................................................................................ 316
A.9
Word structure and address.............................................................................................................................. 324
A.10
Character set ....................................................................................................................................................... 325
A.11
Block format......................................................................................................................................................... 325
A.12
List of instructions ............................................................................................................................................... 327
1
Fundamental safety instructions
1.1
General safety instructions
WARNING
Danger to life if the safety instructions and residual risks are not observed
If the safety instructions and residual risks in the associated hardware documentation are not observed, accidents involving
severe injuries or death can occur.
•
Observe the safety instructions given in the hardware documentation.
•
Consider the residual risks for the risk evaluation.
WARNING
Malfunctions of the machine as a result of incorrect or changed parameter settings
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.
•
Handle possible malfunctions by taking suitable measures, e.g. emergency stop or emergency off.
1.2
Warranty and liability for application examples
The application examples are not binding and do not claim to be complete regarding configuration, equipment or any
eventuality which may arise. The application examples do not represent specific customer solutions, but are only intended to
provide support for typical tasks. You are responsible for the proper operation of the described products. These application
examples do not relieve you of your responsibility for safe handling when using, installing, operating and maintaining the
equipment.
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
9
1.3
Industrial security
Note
Industrial security
Siemens provides products and solutions with industrial security functions that support the secure operation of plants,
systems, machines and networks.
In order to protect plants, systems, machines and networks against cyber threats, it is necessary to implement – and
continuously maintain – a holistic, state-of-the-art industrial security concept. Siemens products and solutions only represent
one component of such a concept.
The customer is responsible for preventing unauthorized access to its plants, systems, machines and networks. Systems,
machines and components should only be connected to the enterprise network or the internet if and to the extent necessary
and with appropriate security measures (e.g. use of firewalls and network segmentation) in place.
Additionally, Siemens’ guidance on appropriate security measures should be taken into account. For more information about
industrial security, please visit:
Industrial security (http://www.siemens.com/industrialsecurity).
Siemens’ products and solutions undergo continuous development to make them more secure. Siemens strongly
recommends to apply product updates as soon as available and to always use the latest product versions. Use of product
versions that are no longer supported, and failure to apply latest updates may increase customer’s exposure to cyber
threats.
To stay informed about product updates, subscribe to the Siemens Industrial Security RSS Feed at:
Industrial security (http://www.siemens.com/industrialsecurity).
WARNING
Unsafe operating states resulting from software manipulation
Software manipulations (e.g. viruses, trojans, malware or worms) can cause unsafe operating states in your system that
may lead to death, serious injury, and property damage.
•
Keep the software up to date.
•
Incorporate the automation and drive components into a holistic, state-of-the-art industrial security concept for the
installation or machine.
•
Make sure that you include all installed products into the holistic industrial security concept.
•
Protect files stored on exchangeable storage media from malicious software by with suitable protection measures, e.g.
virus scanners.
2
Introduction
Note
Chapter "Machining typical milling parts (Page 235)" later in this manual provides you with typical machining examples
including workpiece drawings, typical programs, and step-by-step operating instructions. It helps you to quickly understand
CNC programming and operation through practical examples.
2.1
Panel Processing Units (PPUs)
2.1.1
PPU versions
PPU version Technology variant Operator panel variant
Applicable control system
PPU161.3
Turning variant
Horizontal panel, with English keys
SINUMERIK 808D ADVANCED T (Turning)
Horizontal panel, with Chinese keys
Milling variant
Horizontal panel, with English keys
SINUMERIK 808D ADVANCED M (Milling)
Horizontal panel, with Chinese keys
PPU160.3
Turning variant
Vertical panel, with English keys
SINUMERIK 808D ADVANCED T (Turning)
Vertical panel, with Chinese keys
Milling variant
Vertical panel, with English keys
SINUMERIK 808D ADVANCED M (Milling)
Vertical panel, with Chinese keys
Programming and Operating Manual (Milling)
10
6FC5398-4DP10-0BA6, 09/2017
PPU version Technology variant Operator panel variant
Applicable control system
PPU151.3
Turning variant
Horizontal panel, with English keys
SINUMERIK 808D ADVANCED T (Turning)
Horizontal panel, with Chinese keys
Milling variant
Horizontal panel, with English keys
SINUMERIK 808D ADVANCED M (Milling)
Horizontal panel, with Chinese keys
PPU150.3
Turning variant
Vertical panel, with English keys
SINUMERIK 808D ADVANCED T (Turning)
Vertical panel, with Chinese keys
Milling variant
Vertical panel, with English keys
SINUMERIK 808D ADVANCED M (Milling)
Vertical panel, with Chinese keys
PPU141.3
Turning variant
Horizontal panel, with English keys
SINUMERIK 808D (Turning)
Horizontal panel, with Chinese keys
Milling variant
Horizontal panel, with English keys
SINUMERIK 808D (Milling)
Horizontal panel, with Chinese keys
2.1.2
PPU control elements
①
Status indicators
⑧
Alarm cancellation key
Cancels alarms and messages that are marked with the
symbol on this key
②
Protective cover for USB interface
⑨
Wizard key
Guides you through performing basic commissioning
and operation tasks
③
USB interface
⑩
Help key
Calls help information
④
Horizontal and vertical keys
Call the corresponding vertical/horizontal softkeys on
the screen
⑪
Cursor keys
⑤
Return key
Returns to the next higher-level menu
⑫
Modifier keys for use in key combinations
⑥
Menu extension key
Calls the extended menu items
⑬
Edit control keys
⑦
Alphabetic and numeric keys
⑭
Operating area keys
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
11
Additional information about keys
: Creates a screenshot of the actual user interface
: Saves start-up archives and action logs to a USB stick
: Displays pre-defined slides on the screen
: Saves action logs to a USB stick
Calls the calculator function when you position the cursor on the desired input field
: Changes the screen backlight brightness by an increment of 10% (bright-
ness range: 10% to 100%)
Note that after you release the key combination, the HMI saves your brightness setting and the
brightness bar disappears after a few seconds.
Enters the upper character shown on the alphabetic/numeric keys concerned
+
Opens the system data operating area
In the program editor, pressing this key moves the cursor to the beginning of the selected pro-
gram block.
•
Toggles between entries in the input field
•
Enters the "Set-up menu" dialog box at NC startup
Enables user-defined extension applications, for example, generation of user dialog boxes with
the EasyXLanguage function. For more information about this function, see the SINUMERIK
808D/SINUMERIK 808D ADVANCED Function Manual.
Status indicators
Indicator
Status and meaning
"POK"
•
Solid green: The power supply for the control system is switched on.
"RDY"
•
Solid green: The control system is ready and the PLC is in run mode.
•
Solid red: The control system is in stop mode.
•
Solid orange: The PLC is in stop mode.
•
Flashing orange: The PLC is in power-up mode.
"TEMP"
•
Off: The temperature of the control system is within the specified scope.
•
Solid orange: The temperature of the control system is beyond the scope.
Programming and Operating Manual (Milling)
12
6FC5398-4DP10-0BA6, 09/2017
2.1.3
Screen layout
Alarms and messages in the status area
Displays active alarms with alarm text
The alarm number is displayed in white letter-
ing on a red background. The associated
alarm text is shown in red lettering. An arrow
indicates that several alarms are active. The
number to the right of the arrow indicates the
total number of active alarms. When more
than one alarm is active, the display scrolls
through the alarms in sequence. An acknowl-
edgement symbol indicates the alarm cancel
criterion.
Displays messages from NC programs
Messages from NC programs do not have
numbers and appear in green lettering.
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
13
2.2
Machine Control Panels (MCPs)
2.2.1
MCP versions
MCP version
Applicable control system
•
Horizontal MCP, with English keys and override switches
•
Horizontal MCP, with Chinese keys and override switches
•
Vertical MCP, with English keys and a reserved slot for
the handwheel
•
Vertical MCP, with Chinese keys and a reserved slot for
the handwheel
•
Vertical MCP, with English keys and an override switch
for the spindle
•
Vertical MCP, with Chinese keys and an override switch
for the spindle
All MCP variants are applicable to any of the following
control systems:
•
SINUMERIK 808D ADVANCED T (Turning)
•
SINUMERIK 808D ADVANCED M (Milling)
•
SINUMERIK 808D (Turning)
•
SINUMERIK 808D (Milling)
2.2.2
MCP control elements
Horizontal MCP
Vertical MCP
•
Variant with an override switch for the spindle
•
Variant with a reserved slot for the handwheel
①
Reserved hole for emergency stop button
⑧
Feedrate override switch
②
Tool number display
Displays the number of the currently active tool
⑨
Spindle control keys
Programming and Operating Manual (Milling)
14
6FC5398-4DP10-0BA6, 09/2017
③
Operating mode selection area
⑩
Keys for program start, stop, and reset
④
Program control keys
⑪
Pre-defined labeling strips for keys of the MCP
⑤
User-defined keys
⑫
Reserved slot for the handwheel
⑥
Axis traversing keys
⑬
Spindle override control keys
⑦
Spindle override switch
Functions of user-defined keys
Switches on/off the machine tool working lamp (always active independent of the machine operating
mode)
Indicator on: The working lamp on the machine tool is switched on.
Indicator off: The working lamp on the machine tool is switched off.
Switches on/off of the coolant supply (always active independent of the machine operating mode)
Indicator on: The coolant supply is switched on.
Indicator off: The coolant supply is switched off.
Controls the locking/unlocking of the safety door
Indicator on: The safety door is unlocked.
Indicator off: The safety door is locked.
Note:
If you want to unlock the safety door, make sure all axes and the spindle have stopped running.
Controls if the magazine rotates clockwise (active only when the machine is in "JOG" mode)
Indicator on: The magazine rotates clockwise.
Indicator off: The magazine stops clockwise rotation.
Controls if the magazine approaches the reference point (active only when the machine is in "JOG"
mode)
LED on: The magazine is referenced.
LED off: The magazine is not yet referenced.
Controls if the magazine rotates counter-clockwise (active only when the machine is in "JOG" mode)
Indicator on: The magazine rotates counter-clockwise.
Indicator off: The magazine stops counter-clockwise rotation.
Controls if the chip remover rotates forward (active only when the machine is in "JOG" mode)
Indicator on: The chip remover starts forward rotation.
Indicator off: The chip remover stops rotation.
Controls if the chip remover rotates reversely (active only when the machine is in "JOG" mode)
Indicator on: The chip remover starts reverse rotation.
Indicator off: The chip remover stops reverse rotation.
K9 to K12
Reserved keys.
You can define the functions of these keys in PLC Programming Tool. For more information, see the
SINUMERIK 808D/SINUMERIK 808D ADVANCED Commissioning Manual.
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
15
Pre-defined labeling strips for keys of the MCP
The MCP package includes two sets (six pieces each) of pre-defined labeling strips. One set (① as shown below) is for the
turning variant of the control system and pre-inserted on the back of the MCP. The other set (② as shown below) 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 labeling strips with the milling-
specific ones.
If the pre-defined labeling strips cannot meet your needs, proceed as follows to make customized labeling strips by using the
A4-sized blank plastic sheet in the MCP package:
1. Open the "Symbols for MCP customized key_808D" file in the "\examples\SINUMERIK_808D\MCP" folder on the
Toolbox DVD for the control system on your computer.
2. Copy the desired symbols of keys from the file and then paste them to the desired locations for key labels in the
"Strip_template_808D" file.
3. Print the final labeling strip template file on the blank plastic sheet.
4. Replace the pre-inserted labeling strips from the MCP with the customized ones.
Programming and Operating Manual (Milling)
16
6FC5398-4DP10-0BA6, 09/2017
2.3
Coordinate systems
As a rule, a coordinate system is formed from three mutually perpendicular coordinate axes. The positive directions of the
coordinate axes are defined using the Cartesian coordinate system. The coordinate system is related to the workpiece and
programming takes place independently 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 respective machine types. It can be rotated
in different positions.
The directions of the axes follow the Cartesian coordinate system.
The figure below shows an example of the machine coordinate system of a flat-body turning machine with a front tool holder.
The origin of this coordinate system is the m achine zero, defined by the machine manufacturer.
The traversing range of the m achine axes can be in the negative range.
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
17
Workpiece coordinate system (WCS)
To describe the geometry of a workpiece in the workpiece program, a right-handed, right-angled coordinate system is also
used.
Generally, X0/Y0 of the WCS is set at the center, edge or corner of the workpiece while Z0 is set on the top surface of the
workpiece.
See the following illustrations for X0/Y0 at the center, edge and corner of the workpiece respectively.
The figure below shows an example of the workpiece coordinate system.
Relative coordinate system (REL)
In addition to the machine and workpiece coordinate systems, this control system provides a relative coordinate system.
This coordinate system can clear the current coordinate values at any position and has no influence on workpiece machining
or the position of WCS. All axis movements are displayed relative to this position.
Programming and Operating Manual (Milling)
18
6FC5398-4DP10-0BA6, 09/2017
2.4
Protection levels
Overview
The control system provides a concept of protection levels for enabling data areas. Different protection levels control
different access rights.
The control system delivered by Siemens is set by default to the lowest protection level 7 (without password). If the
password is no longer known, the control system must be reinitialized with the default machine/drive data. All passwords are
then reset to default passwords for this software release.
Note
Before you boot the control system with default machine/drive data, make sure that you have backed up your machine/drive
data; otherwise, all data are lost after rebooting with default machine/drive data.
Protection level
Locked by
Area
0
Siemens password
Siemens, reserved
1
Manufacturer password
Machine manufacturers
2
Reserved
-
3-6
End user password
(Default password: "CUSTOMER")
End users
7
No password
End users
Protection level 1
Protection level 1 requires a manufacturer password. With this password entry, you can perform the following operations:
● Entering or changing part of the machine data and drive data
● Conducting NC and drive commissioning
Protection level 3-6
Protection level 3-6 requires an end user password. With this password entry, you can perform the following operations:
● Entering or changing part of the machine data
● Editing programs
● Setting offset values
● Measuring tools
Protection level 7
If you have not set the password or protection level interface signal, the system sets the protection level to 7 automatically.
With this password entry, you can perform the following operations:
● Editing programs
● Setting offset values
● Measuring tools
You can also set protection level 7 through the PLC user interfaces. For more information, see the
SINUMERIK 808D/SINUMERIK 808D ADVANCED Commissioning Manual.
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...).
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
19
Setting the password
+
1.
Select the system data operating area.
2.
Open the following password setting window and then enter the desired password (default
end-user password: CUSTOMER):
3.
Confirm the input.
Changing/deleting the password
Note
To avoid unauthorized access to the controller, you must change the Siemens default passwords to your own ones.
+
1.
Select the system data operating area.
2.
If you desire to change the existing password, press this softkey to open the following win-
dow and enter the new password:
If you desire to delete the existing password, proceed directly to Step 6.
3.
Confirm the new password.
4.
Enter the new password again in the following window:
5.
Press this softkey to confirm the new password.
6.
If you desire to delete the existing password, directly press this softkey.
Programming and Operating Manual (Milling)
20
6FC5398-4DP10-0BA6, 09/2017
3
Common notices for machining operations
To ensure the safety and correctness of machining, you must observe the following notices during machining operations:
● Reference point approach is required only for machine tools equipped with incremental encoders.
● Before running the spindle manually, make sure you have activated the tool.
● Before executing M functions, make sure all the axes are in safe positions.
● During handwheel assignment, make sure there is no obstacle when moving the tool to avoid tool collision.
● To guarantee the safety and correctness of machining, you must verify the tool setup result.
● You must distinguish the direction of tool wear compensation clearly before entering the tool wear offsets.
● Before machining the workpiece on the machine, make sure the following preconditions are met:
– The PRT mode and the dry run feedrate are deactivated.
– The feedrate override is 0%.
– The safety door is closed.
● After changing important data, it is recommended to carry out an internal data backup immediately.
4
Switching on and referencing
Note
Reference point approach is required only for machine tools equipped with incremental encoders.
Operating sequence
1.
Turn on the power supply for the machine tool.
2.
Release all emergency stop buttons on the machine. By default, the control system is in
reference point approach (REF.POINT) mode after startup.
•
If a machine axis is equipped with an absolute encoder, the axis is referenced
automatically after the control system starts and therefore reference point approach is
unnecessary. The circle symbol (lower-left figure) next to the axis identifier indicates that
the axis is already referenced.
•
If a machine axis is equipped with an incremental encoder, the axis is not referenced
after the control system starts. The circle symbol (lower-right figure) next to the axis
identifier indicates that the axis has not been referenced. Proceed to Step 3.
3.
Use the corresponding axis traversing keys to traverse the axes until the
symbol appears
next to the axis identifier.
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
21
5
Setting the user interface language
Note
The default user interface language is dependent on the PPU type. For a PPU with Chinese keys, the default language is
Chinese after power-on; otherwise it's English. If you desire to change it, proceed through the following operating sequence;
otherwise, skip this chapter and proceed to the next chapter for setting up tools.
Operating sequence
+
1.
Select the system data operating area.
2.
Open the user interface language selection window.
3.
Use the cursor keys to select the desired language.
4.
Press this softkey to confirm your selection and the system is automatically restarted to
activate the selected language.
6
Setting up tools
6.1
Creating a tool
Note
The control system supports a maximum of 64 tools and 128 cutting edges. You can create a maximum of nine cutting
edges for each tool. Before executing a part program, you must first create the desired tool in the tool list and proceed with
the tool setting operations.
Operating sequence
1.
Select the offset operating area.
2.
Open the tool list window.
3.
Open the lower-level menu for tool type selection.
Programming and Operating Manual (Milling)
22
6FC5398-4DP10-0BA6, 09/2017
4.
Select a tool type (for example, a milling tool) with the corresponding softkey.
5.
Enter the tool number in the following window:
6.
Press this softkey to confirm your settings. The window below shows the information of the
new tool created. Set the desired tool data in this window.
•
Column ① indicates the tool offset number in Siemens dialect mode.
•
Column ② indicates the tool offset number visible only in ISO dialect mode.
7.
Press this key to confirm your settings.
6.2
Creating/changing a cutting edge
Note
Before creating or changing cutting edges, you must first create tools (Page 21).
Operating sequence
1.
Select the offset operating area.
2.
Open the tool list window.
3.
Select the tool to which you desire to add a cutting edge.
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
23
4.
Open the menu items for cutting edge settings.
5.
Press this softkey to create a new cutting edge for the selected tool. The control system
automatically adds the new cutting edge to the tool list. Now you can enter different
lengths and radii for each cutting edge.
6.
You can also press the corresponding softkey to reset or delete a cutting edge.
6.3
Activating the tool and the spindle
Note
A tool in the tool list is not active until you activate it in "MDA" mode or the "T, S, M" window.
Operating sequence
1.
Select the machining 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.
Programming and Operating Manual (Milling)
24
6FC5398-4DP10-0BA6, 09/2017
5.
Press this key to move the cursor to the input field for the spindle speed, and enter the de-
sired speed, for example, 1000.
6.
Press this key again to move the cursor to the input field for the spindle direction.
7.
Use this key to select the spindle direction, for example, "M3".
8.
Press this key on the MCP to activate the tool and the spindle.
9.
Press this key on the MCP to stop spindle rotation.
10.
Press this softkey to return to the main screen of the machining operating area.
Note
You can alternatively activate the spindle using the following keys on the MCP:
/
For more information, see Section "Running the spindle manually (Page 288)".
6.4
Assigning the handwheel
If the machine manufacturer has assigned the handwheel for the control system, you can skip this section and directly
measure the tool (Page 27) after activating the tool and the spindle (Page 23).
This control system provides the following two methods for assigning the handwheel:
● Assigning the handwheel through the MCP (Page 24)
● Assigning the handwheel through the PPU (Page 25)
Note
Make sure there is no obstacle when moving the tool to avoid tool collision.
6.4.1
Assigning the handwheel through the MCP
Precondition
MD14512[16].7 = 0 (factory default)
Operating sequence
1.
Select the machining operating area.
2.
Press this key on the MCP to control the axis movement with external handwheels.
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
25
3.
Press the desired axis traversing keys to assign the handwheel.
4.
Press the increment keys on the MCP to select the required override increment.
•
1: The override increment is 0.001 mm.
•
10: The override increment is 0.010 mm.
•
100: The override increment is 0.100 mm.
5.
Rotate the handwheel to make the selected axis approach the workpiece.
6.
Cut the surface of the workpiece to verify the handwheel assignment.
7.
Press this softkey to close the window for handwheel assignment.
8.
Press this key to return to the main screen of the machining operating area.
6.4.2
Assigning the handwheel through the PPU
Precondition
Set MD14512[16].7 = 80 (default value: 0). With this setting, you can only assign the handwheel through the PPU.
Operating sequence (activating the handwheel control function on the PPU)
If this function is already active, skip the steps below and proceed directly to the operating sequence for assigning the
handwheel through the PPU.
+
1.
Select the system data operating area.
2.
Open the machine data window.
3.
Press this softkey to open the basic machine data list.
4.
Press this softkey to open the search field and enter the machine data "14512".
5.
Confirm your entry with this softkey. Then the system starts searching automatically.
6.
Move the cursor to the input field for 14512[16].
7.
Enter the value "80".
8.
Confirm your entry.
9.
Press this vertical softkey to activate the value change. Note that the control system restarts
to accept the new value.
Programming and Operating Manual (Milling)
26
6FC5398-4DP10-0BA6, 09/2017
Operating sequence (assigning the handwheel through the PPU)
1.
Select the machining operating area.
2.
Press this key on the MCP.
3.
Press this key to open the extended menu.
4.
Open the handwheel assignment window.
5.
Select the handwheel to be assigned with the cursor keys in the following window. You can
assign a maximum of two handwheels.
6.
Press the desired vertical softkey ( ... ) or this key for the handwheel assignment.
The handwheel symbol which appears to the left of the selected axis (for example, the X-
axis) indicates that you have assigned the handwheel to the selected axis.
7.
Press the increment keys on the MCP to select the required override increment.
•
1: The override increment is 0.001 mm.
•
10: The override increment is 0.010 mm.
•
100: The override increment is 0.100 mm.
8.
Rotate the handwheel to make the selected axis approach the workpiece.
9.
Machine a surface to verify the handwheel assignment.
10.
Press this softkey to close the window for handwheel assignment.
11.
Press this key to return to the main screen of the machining operating area.
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
27
6.5
Measuring the tool manually
Note
•
You must first create a tool (Page 21) and activate it (Page 23) before measuring the tool.
•
This section takes the milling tool measurement for example. If you have created other types of tools, proceed through
the following steps to finish the measurement of all the tools. This will make the tool change process easier.
Operating sequence
1.
Select the machining operating area.
2.
Switch to "JOG" mode.
3.
Open the tool measurement window.
4.
Open the manual tool measurement window.
5.
Press the axis traversing keys to move the infeed axes to the desired positions above the
workpiece.
6.
Switch to handwheel control mode.
7.
Press this key to set the workpiece or a fixed point as the reference point.
Note:
You can define a fixed point as desired, for example, the workbench.
8.
Select a suitable override feedrate, and then use the handwheel to move the tool to scratch
the required workpiece edge (see the left illustration shown below) or the edge of the setting
block, if it is used (see the right illustration shown below).
9.
Enter the distance between the tool tip and the reference point in the "Z0" field, for example,
"0". (This value is the thickness of a setting block if it is used.)
10.
Save the tool length value in the Z axis. The tool diameter, radius, and cutting edge position
are all taken in to account.
11.
Press this vertical softkey to open the window for measuring the tool diameter.
12.
Press the axis traversing keys to move the tool to approach the workpiece in the X direction.
Programming and Operating Manual (Milling)
28
6FC5398-4DP10-0BA6, 09/2017
13.
Switch to handwheel control mode.
14.
Select a suitable override feedrate, and then use the handwheel to move the tool to scratch
the required workpiece edge (or the edge of the setting block, if it is used).
15.
Enter the distance to the workpiece edge in the X and Y directions in the "X0" and "Y0"
fields respectively, for example, enter "0" at "X0" and "0" at "Y0". (This is the value of the
width of a setting block if it is used. Select one of X0/Y0 as required.)
16.
Save the tool diameter value.
17.
Press this softkey and you can see that the compensation data values have been automati-
cally added to the tool data.
6.6
Verifying the tool offset result
To guarantee the safety and correctness of machining, you must verify the tool setup result.
Note
Before verifying the tool setup result, you must have finished all tool setup work as mentioned before.
Operating sequence
1.
Select the machining operating area.
2.
Switch to "MDA" mode.
3.
Press this softkey on the PPU.
4.
Enter the following test program (or you can create your own program):
T1 D1
G00 X0 Y0 Z5
Alternatively, you can press this softkey to load an existing part program from a system
directory.
5.
Press this key to activate the "ROV" function (indicator on: this function is active).
Note:
After the "ROV" function is active, the feedrate override switch can also control the speed of
G00.
6.
Rotate the feedrate override switch to 0%.
7.
Press this key on the MCP.
Increase the feedrate override gradually to avoid accidents caused by fast axis movement.
Observe whether the axis moves to the specified position.
For more information on the further softkey functions in "MDA" mode, see Section ""MDA" mode (Page 295)".
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
29
7
Creating part programs
7.1
Creating a part program
The control system can store a maximum of 300 part programs which include those created by the control system for certain
functions such as MM+, TSM, and so on.
WARNING
Machine malfunction due to use of insecure part programs
Running an insecure part program on your machine may cause unexpected attacks to the machine, which in turn can lead
to death, personal injuries, and/or machine damage.
•
Make sure that you use part programs that come from trusted sources.
Methods for creating part programs
You can create a part program with one of the following methods:
● Creating on a computer and transferring it to the PPU via USB interface (Page 67)
● Creating on a computer and transferring it to the PPU via Ethernet interface (Page 70)
● Creating directly on the PPU (see below for details)
Creating a part program on the PPU
1.
Select the program management operating area.
2.
Press this softkey to enter the system directory for storing part programs.
3.
To directly create a new program file, press this softkey and go to Step 4.
To create a new program directory first, press this softkey and proceed as follows before
you go to Step 4:
A. Press this softkey to open the window for creating a new directory.
B. Enter a desired name for the new directory. Note that some special characters (see table
at the end of this section) are invalid for the directory name.
C. Press this softkey to confirm your entry.
D. Select the new directory with the cursor keys.
E. Press this key on the PPU to open the directory.
Programming and Operating Manual (Milling)
30
6FC5398-4DP10-0BA6, 09/2017
4.
Press this softkey to open the window for creating a new program.
5.
Enter the name of the new program. You can enter the file name extension ".MPF" (main
program) or ".SPF" (subprogram) to define the program type. The control system identifies a
program as a main program if you do not enter any file name extension. The character
length of a program name is limited to 24 English characters or 12 Chinese characters. Note
that some special characters (see table at the end of this section) are invalid for the pro-
gram name.
6.
Press this softkey to confirm your entry. The part program editor window opens automatical-
ly. Now you can edit the program text in the window. The control system saves your editing
automatically.
Special characters invalid for program or directory names
The control system does not support the use of the following special characters in program or directory names:
/
<
>
?
:
#
(
)
[
]
$
!
-
+
^
\
*
|
;
&
%
@
=
~
`
Space
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
31
7.2
Editing the part program
7.2.1
Using a standard program structure
Using a standard program structure provides an easy way of part programming and a clear view of the machining
sequences. Siemens recommends that you use the following program structure:
7.2.2
Editing a part program
Methods for editing part programs
You can edit a part program with one of the following methods:
● Editing on a computer and transferring it to the PPU via USB interface (Page 67)
● Editing on a computer and transferring it to the PPU via Ethernet interface (Page 70)
● Editing directly on the PPU (see below for details)
Editing an internal part program on the PPU
You can edit an internal part program only when it is not being executed. Note that any modification to the part program in
the program editor window is stored immediately.
Note:
Steps 1 to 4: Search for a program file
Steps 5 to 9: Edit the selected program in the open program editor window
1.
Select the program management operating area.
2.
Press this softkey to enter the system directory for storing part programs.
Programming and Operating Manual (Milling)
32
6FC5398-4DP10-0BA6, 09/2017
3.
Select the desired program file/directory in one of the following methods:
•
Navigate to the program/directory with the cursor keys
•
Open the search dialog box and enter the desired search term.
Note:
If you search for a program, the file name extension must be entered in the first input
field of the dialog box below.
•
On the PPU, press the alphabetic or numeric key that contains the first character of the
desired program/directory name. The control system automatically highlights the first
program/directory whose name starts with that character. If necessary, press the key
continuously until you find the desired program/directory.
4.
Press this key to open either the selected program in the program editor or the selected
directory. In the latter case, perform Step 3 and then Step 4 until the selected program is
opened in the program editor.
5.
Edit the program text in the program editor window using the following keys on the PPU:
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
33
6.
When necessary, select the following vertical softkeys to complete more program editing
operations.
•
Renumbering program blocks
With this softkey, you can modify the block numbering (Nxx) of a program opened in the
program editor window. After you press this softkey, the block number is inserted at the
beginning of the program block in ascending order and is increased by an increment of 10
(for example, N10, N20, N30).
•
Searching in programs
Pressing this softkey opens the search dialog box. You can use the search function to
quickly arrive at points where you would like to make changes, for example, in very large
programs. You can search with specified text or line number by selecting the corresponding
softkey as follows:
•
Copying/deleting/pasting program blocks
A. Press this softkey in the open program editor window to insert a marker.
B. Select the desired program blocks with the cursor.
C. Press this softkey to copy the selection to the buffer memory.
- OR -
Press this key to delete the selected program blocks and to copy them into the buffer
memory.
Programming and Operating Manual (Milling)
34
6FC5398-4DP10-0BA6, 09/2017
D. Place the cursor on the desired insertion point in the program and press this softkey. The
content of the buffer memory is pasted.
7.
If you want to program cycles, press the corresponding softkey to open the desired cycle
programming window. For more information, see Section "Cycles (Page 152)".
8.
If you want to program contours, press this softkey to open the contour programming win-
dow. For more information, see Section "Free contour programming (Page 306)".
9.
Press this key to return to the program management operating area after finishing editing.
Note:
When you are in the main screen of the program management operating area, you can
select to make the following operations between programs:
•
Searching for programs
•
Copying/cutting/pasting programs
•
Deleting/restoring programs
•
Renaming programs
For more information, see Section "Program management operating area (Page 281)".
Editing an external part program on the PPU
You can edit an external part program directly on the PPU. Note that the program can be edited only when it is not being
executed.
Note:
Steps 1 to 3: Search for a program file
Steps 4 to 7: Edit the selected program in the open program editor window
1.
Select the program management operating area.
2.
Press the desired softkey to enter the target program directory.
3.
Follow the above steps 3 and 4 for editing an internal program to search for and open the
desired program file.
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
35
4.
Edit the program text in the program editor window using the following keys on the PPU:
5.
When necessary, select the following vertical softkeys to complete more program editing
operations.
•
Renumbering program blocks
With this softkey, you can modify the block numbering (Nxx) of a program opened in the
program editor window. After you press this softkey, the block number is inserted at the
beginning of the program block in ascending order and is increased by an increment of 10
(for example, N10, N20, N30).
•
Searching and replacing in programs
Pressing this softkey opens the search dialog box. You can use the search function to
quickly arrive at points where you would like to make changes, for example, in very large
programs.
You can search with specified text or line number by selecting the corresponding softkey as
follows:
If more than one search result is found, you can also use the following softkey to check the
remaining results one by one:
You can search and replace with specified text by using the following softkey:
If more than one search result is found, you can also use the following softkey to replace the
remaining results one by one:
•
Copying/deleting/pasting program blocks
A. Press this softkey in the open program editor window to insert a marker.
B. Select the desired program blocks with the cursor.
Programming and Operating Manual (Milling)
36
6FC5398-4DP10-0BA6, 09/2017
C. Press this softkey to copy the selection to the buffer memory.
- OR -
/
Press this key/softkey to delete the selected program blocks and to copy them into the buff-
er memory.
D. Place the cursor on the desired insertion point in the program and press this softkey. The
content of the buffer memory is pasted.
•
Cutting a row of program blocks
With this softkey, you can delete the entire program row where the cursor is placed and
copy into the buffer memory. Then you can move the cursor to the desired position and
press the following softkey to paste the cut program row at the current cursor position:
•
Undoing/redoing operations
Pressing this softkey allows you to revoke your last operation.
Pressing this softkey allows you to restore your last operation that is revoked.
6.
Save the program file after finishing editing through the following softkey operations:
→
If you switch to any other operating area after finishing editing without saving, a message
appears to remind you to save the file, for example:
In this case, you may press either of the following softkeys as desired:
Pressing this softkey aborts the editing results and system switches to the desired operating
area.
Pressing this softkey saves the editing results before the system switches to the desired
operating area.
7.
Press this key to return to the program management operating area.
Note:
When you are in the main screen of the program management operating area, you can
select to make the following operations between programs:
•
Searching for programs
•
Copying/cutting/pasting programs
•
Deleting programs
•
Renaming programs
For more information, see Section "Program management operating area (Page 281)".
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
37
Note
When you perform editing operations such as renumbering, searching, and saving of an external program file larger than
4 MB, a message appears reminding you that it will take a long time to complete the operations.
To ensure that the program editor works properly, you are recommended to edit an external program file smaller than
200 MB.
7.2.3
Understanding frequently used programming instructions
7.2.3.1
Inch or metric dimensions (G70/G71)
Description
Programming example
G71:
With G71 at the program start, both the geometrical data
and the feedrates are evaluated as metric units.
N10 G17 G90 G54 G71
N20 T1 D1 M6
N30 S5000 M3 G94 F300
N40 G00 X100 Y100 Z5
N50 G01 Z-5
N60 Z5
N70 G00 Z500 D0
G70:
With G70 at the program start, the geometrical data is eval-
uated as inches, but the feedrates are not affected and
remain as metric units.
N10 G17 G90 G54 G70
N20 T1 D1 M6
N30 S5000 M3 G94 F300
N40 G00 X3.93 Y3.93 Z5
N50 G01 Z-0.787
N60 Z0.196
N70 G00 Z19.68 D0
For more information, see Section "Dimensions in metric units and inches: G71, G70, G710, G700 (Page 82)".
7.2.3.2
Definition of work offset (G54 to G59, G500, G90/G91)
Description
Illustration
Programming example
G500:
All absolute path data corresponds to
the current position. The position val-
ues are written in the G500 (basic) zero
offset.
N10 G17 G90 G500 G71
N20 T1 D1 M6
N30 S5000 M3 G94 F300
N40 G00 X50 Y50 Z5
N50 G01 Z-20
N60 Z5
N70 G00 Z500 D0
G54 to G59:
With G500 = 0, the offset for the work-
piece can be stored in the workpiece
offsets G54 to G59.
N10 G17 G90 G54 G71
N20 T1 D1 M6
N30 S5000 M3 G94 F300
N40 G00 X0 Y0 Z5
N50 G01 Z-20
N60 Z5
N70 G00 Z500 D0
Programming and Operating Manual (Milling)
38
6FC5398-4DP10-0BA6, 09/2017
Description
Illustration
Programming example
G500 + G54:
With G500 ≠ 0 activated, the value in
G500 is added to the value in G54.
N10 G17 G90 G500 G71
N20 T1 D1 M6
N30 S5000 M3 G94 F300
N40 G00 G54 X20 Y20 Z5
N50 G01 Z-20
N60 Z5
N70 G00 G53 Z500 D0
G90:
With G90 (absolute positioning) at the
program start, the geometrical data
refers to the zero of the coordinate
system currently active in the program,
usually with G54, G500, or G500 +
G54.
-
N10 G17 G90 G54 G71
N20 T1 D1 M6
N30 S5000 M3 G94 F300
N40 G00 X100 Y100 Z5
N50 G01 Z-20
N60 Z5
N70 G00 Z500 D0
G91:
With G91 (incremental positioning), you
can add numerical value of path infor-
mation (the incremental positioning with
the current axis position as the start
point) in the program. Subsequently,
switch to absolute positioning with G90.
-
N10 G17 G90 G54 G70
N20 T1 D1 M6
N30 S5000 M3 G94 F300
N40 G00 X3.93 Y3.93 Z0.196
N50 G01 G91 Z-0.787
N60 Z0.196
N70 G00 G90 Z19.68 D0
For more information, see Sections "Workpiece coordinate system - settable work offset: G54 to G59, G500, G53, G153
(Page 88)" and "Absolute/incremental dimensioning: G90, G91, AC, IC (Page 81)".
7.2.3.3
Rapid traverse (G00)
Description
Illustration
Programming example
G00:
When G00 is active in the program, the
axis will traverse at the maximum axis
speed in a straight line.
Straight line in any direction
N10 G17 G90 G54 G71
N20 T1 D1 M6
N30 S5000 M3 G94 F300
N40 G00 X50 Y50 Z5
N50 G01 Z-5
N60 Z5
N70 G00 Z500 D0
For more information, see Section "Linear interpolation with rapid traverse: G0 (Page 91)".
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
39
7.2.3.4
Tool and traverse (T, D, M6, F, G94/G95, S, M3/M4, G01)
Description
Programming example
T, D:
A new tool can be selected with the "T" command, and the "D" command
is used to activate the tool length offset.
M6:
M6 can be used for automatic tool change on the machine.
G94/G95, F:
The feedrate is defined with "F". G94 F defines feedrate in terms of time
(mm/min) and G95 F defines feedrate in terms of spindle revolutions
(mm/rev).
S, M3/M4:
The spindle speed is defined with "S". The spindle direction is defined
with M3(clockwise) and M4 (counter-clockwise).
G01:
When G01 is active in the program, the axis traverses at the pro-
grammed feedrate (as defined by G94 F or G95 F) in a straight line.
N10 G17 G90 G54 G71
N20 T1 D1 M6
N30 S5000 M3 G94 F300
N40 G00 X50 Y50 Z5
N50 G01 Z-5
N60 Z5
N70 G00 Z500 D0
For more information, see sections as follows:
● Tool T (Page 116)
● Tool compensation number D (Page 116)
● Feedrate F (Page 92)
● Spindle speed S, directions of rotation (Page 109)
● Linear interpolation with feedrate: G1 (Page 92)
7.2.3.5
Tool radius compensation (G40, G41/G42)
The tool radius compensation can be activated (G41/G42) or deactivated (G40) in contour programming.
● G41: tool radius compensation to the left of the contour
● G42: tool radius compensation to the right of the contour
● G40: tool radius compensation off
When traversing circle contours with cutter radius compensation, it must be decided whether the feedrate should act at the
circle contour of the workpiece (CFC) or the path defined by the cutter center point (CFTCP).
When using the feedrate at the circle contour defined by the CFC command, the feedrate is constant at the contour, which
however may cause increase in the feedrate of the tool. This increase could damage the tool if excessive material is
encountered at the contour. Therefore, CFC is commonly used for finish cutting of contours.
The CFTCP command ensures a constant feedrate of the tool, but different feedrates at the contour. This may cause
deviations in surface finish.
Programming and Operating Manual (Milling)
40
6FC5398-4DP10-0BA6, 09/2017
These two commands may cause the cutter to traverse fast around a corner or slowly at the contour.
For more information, see Sections "Tool radius compensation OFF: G40 (Page 122)" and "Selecting the tool radius
compensation: G41, G42 (Page 119)".
7.2.3.6
Milling circles and arcs (G02/G03)
The following gives an example of machining arc with specified program code:
N10 G17 G90 G500 G71
N20 T1 D1 M6
N30 S5000 M3 G94 F300
N40 G00 X-20 Y-20 Z5
N50 G01 Z-5
N60 G41 X0 Y0
N70 Y50
N80 X100
N90 G02 X125 Y15 I-12 J-35
N100 G01 Y0
N110 X0
N120 G40 X-20 Y-20
N130 G00 Z500 D0
* Note that N90 block as above can also be written as "N90 G02 X125 Y15 CR=37".
When milling circles and arcs, you must define the circle center point and the distance between the start point, end point,
and the center point in the relative coordinate system.
When using the XY coordinate system, the interpolation parameters I and J are available.
There are two common ways of defining circles and arcs:
● G02/G03 X... Y... I... J...
● G02/G03 X... Y... CR=...
Use positive value in CR with arcs ≤ 180°, and negative value with arcs > 180°.
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
41
SP
Start point of circle
CP
Center point of circle
EP
End point of circle
I
Incremental distance from SP to CP in X axis
J
Incremental distance from SP to CP in Y axis
G2
Traversing direction of the circle (clockwise)
G3
Traversing direction of the circle (counter-clockwise)
For more information, see Section "Circular interpolation: G2, G3 (Page 93)".
7.2.3.7
Fixed point approach (G74/G75)
Description
Programming example
G74:
By using G74, reference point can be approached automati-
cally.
N10 G17 G90 G500 G71
N20 T1 D1 M6
N30 S5000 M3 G94 F300
N40 G00 X50 Y50 Z5
N50 G01 Z-5
N60 Z5
N70 G74 Z=0 ;reference point
G75:
By using G75, a fixed point on the machine defined by the
manufacturer can be approached automatically.
N10 G17 G90 G500 G71
N20 T1 D1 m6
N30 S5000 M3 G94 F300
N40 G00 X50 Y50 Z5
N50 G01 Z-5
N60 Z5
N70 G74 Z=0 ;reference point
N80 G75 X=0 ;fixed point
For more information, see Section "Fixed point approach (Page 104)".
Programming and Operating Manual (Milling)
42
6FC5398-4DP10-0BA6, 09/2017
7.2.3.8
Spindle control
Description
Programming example
M3:
Spindle accelerates to the programmed speed in clockwise
direction.
M4:
Spindle accelerates to the programmed speed in counter-
clockwise direction.
M5:
Spindle decelerates to stop.
M19:
Sets the spindle to a specific angular position.
N10 G17 G90 G500 G71
N20 T1 D1 M6
N30 S5000 M3 G94 F300
N40 G00 X50 Y50 Z5
N50 G01 Z-5
N60 M5
N70 Z5 M4
N80 M5
N90 M19
N100 G00 Z500 D0
For more information, see Section "Spindle movements (Page 109)".
7.2.3.9
Setting dwell time in the program (G04)
Description
Programming example
G04:
G04 can be used to pause the tool movements during ma-
chining process.
G04 F5: program dwells for 5 seconds
This makes the workpiece surface much smoother.
N10 G17 G90 G500 G71
N20 T1 D1 M6
N30 S5000 M3 G94 F300
N40 G00 X50 Y50 Z5
N50 G01 Z-5
N60 G04 F5
N70 Z5 M4
N80 M5
N90 M19
N100 G00 Z500 D0
For more information, see Section "Dwell time: G4 (Page 108)".
8
Program simulation
Simulation before machining
Before automatic machining, you need to perform the simulation to check whether the tool moves in the right way. During
simulation, the current program is calculated in its entirety and the result displayed in graphic form. The result of
programming is verified without traversing the machine axes. Incorrectly programmed machining steps are detected at an
early stage and incorrect machining on the workpiece prevented.
You can choose one of the following methods for simulation:
● Simulation prior to machining of the workpiece (Page 43)
● Simultaneous recording prior to machining of the workpiece (Page 45)
Simulation during machining
If the view of the work space is blocked by coolant, for example, while the workpiece is being machined, you can track the
program execution on the screen. For more information, see Section "Simultaneous recording during machining of the
workpiece (Page 48)".
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
43
8.1
Simulation prior to machining of the workpiece
Before machining the workpiece on the machine, you have the option of performing a quick run-through in order to
graphically display how the program is executed. This provides a simple way of checking the result of the programming.
Operating sequence
Note that the following Steps 1 to 3 describe how to open a desired program file on the
PPU. If you are already in the program editor window, you can go to Step 4 directly.
1.
Select the program management operating area.
2.
Enter the system program directory and position the cursor on the program to be simulated.
3.
Press this key and the program is opened in the program editor window.
4.
Switch to "AUTO" mode.
5.
Press this softkey to open the program simulation window, and the program control mode
PRT is automatically activated.
6.
Press this key to start the simulation for the selected program.
The program execution is displayed graphically on the screen. The machine axes do not
move.
7.
You can also select the vertical softkeys as required in the simulation window as follows:
Scales the entire simulation track automatically to adapt to the size of the window
Programming and Operating Manual (Milling)
44
6FC5398-4DP10-0BA6, 09/2017
Opens the lower-level menu for the following block display options:
•
Display all G17 blocks
•
Display all G18 blocks
•
Display all G19 blocks
Zooms in the screen from the cursor position
Zooms out the screen from the cursor position
Deletes all the simulation tracks recorded up till now
Makes the cursor move in large or small steps
Enables the material removal simulation of a defined blank
Selects whether to show the blocks or not
8.
Press this key on the MCP if you wish to stop the simulation.
- OR -
Press this key on the MCP to cancel the simulation.
9.
Press this key on the MCP to restart or continue the simulation.
10.
After you finish the simulation, you can press this softkey to return to the program editor
window.
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
45
8.2
Simultaneous recording prior to machining of the workpiece
Before machining the workpiece on the machine, you can graphically display the execution of the program on the screen to
monitor the result of the programming.
Operating sequence
1.
Select the program management operating area.
2.
Enter the target program directory and position the cursor on the desired program.
3.
Press this softkey and the system automatically changes to "AUTO" mode in the machining
operating area.
4.
Press this softkey to open the lower-level menu for program control.
5.
Press this softkey to activate the PRT mode, and the program is executed without axis
movement.
You can additionally press this softkey to replace the programmed feedrate with a dry run
feedrate. For more information about setting the dry run feedrate, see Section "Dry run
feedrate (Page 53)".
6.
Press this softkey to open the simultaneous recording window.
7.
Press this key to start the recording. The program execution is displayed graphically on the
screen. The machine axes do not move.
8.
Press this key on the MCP if you wish to stop the recording.
- OR -
Press this key on the MCP to cancel the recording.
9.
Press this key on the MCP to restart or continue the recording.
Note
You must deactivate the PRT mode and the dry run feedrate activated in Steps 4 and 5 above before machining the
workpiece on the machine; otherwise the machining cannot be performed due to the standstill of the axes and the spindle.
For more information about the softkeys in the simultaneous recording window, see Section "Simulation prior to machining of
the workpiece (Page 43)".
Programming and Operating Manual (Milling)
46
6FC5398-4DP10-0BA6, 09/2017
9
Machining the workpiece
9.1
Executing a part program
Before starting a program, make sure that both the control system and the machine are set up, and the part program is
verified with simulation and test. Observe the relevant safety notes of the machine manufacturer.
1.
Select the program management operating area.
2.
Select the desired program directory.
3.
Select the program that you desire to execute.
4.
Press this softkey. For some directories, press the following softkey instead:
The system automatically changes to "AUTO" mode in the machining operating area after
you press the softkey.
5.
If desired, you can use this softkey to specify how you want the program to be executed (for
more information, see Section "Program control functions (Page 53)").
6.
Make sure the feedrate override is 0%. Press this key on the MCP to close the safety door.
If this function is not available, close the door on the machine manually.
7.
Press this key on the MCP to start the machining of the program.
8.
Turn the feedrate override switch slowly to the desired value.
Pressing this key stops the execution of a part program. The program currently running is
aborted. On the next program start, the machining starts from the beginning.
Pressing this key suspends the execution of a part program. The axes stop running while
the spindle continues running. Press the following key again, and the program continues to
run.
Note
To ensure the shortest machining time, do not perform the HMI operations during program running, for example, creating a
new program or editing an external program on the PPU.
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
47
9.2
Executing specified blocks
If you would only like to perform a certain section of a program on the machine, then you do not need to start the program
from the beginning. You can start the program from a specified program block in the following cases:
● After you stop or interrupt the program execution
● When you need to specify a target position, e.g. during remachining
Operating sequence
Proceed as follows to start machining from the last interruption point in the program:
1.
Select the machining operating area.
2.
Switch to "AUTO" mode.
3.
Press this softkey to open the block search window.
4.
Press this softkey to load the interruption point, and the cursor moves to the beginning of
the target block which is interrupted last time.
5.
Press one of the following softkeys to set the condition for the block search:
•
The program will continue from the line before the target block. The same calculations of
the basic conditions (e.g. tool and cutting edge numbers, M functions, feedrate and
spindle speed) in the previous blocks are carried out as during normal program
operation, but the axes do not move.
•
The program will continue from the target block containing the interruption point. The
same calculations of the basic conditions in the previous blocks are carried out as during
normal program operation, but the axes do not move.
•
Block search without calculation of the basic conditions. All settings required for
execution have to be programmed from the target block (e.g. feedrate, spindle speed,
etc.).
For the block search to contour/end point, make sure you set MD11450 bit 2 to 1 to sup-
press the output of the auxiliary functions. Note that MD11450 is visible only with the manu-
facturer password.
6.
Make sure the feedrate override is 0%.
7.
Press this key on the MCP, and then an alarm 010208 appears for your confirmation
whether to continue.
8.
Press this key again to execute the program.
9.
Turn the feedrate override switch on the MCP slowly to the desired value.
NOTICE
Damage to workpiece or machine tools
For the machining in ISO mode, you must program the desired feedrate from the target block after a block search without
calculation. Otherwise, the axis will traverse at the maximum speed with G0 after you execute the program, which may
cause damage to the workpiece or the machine tools.
Programming and Operating Manual (Milling)
48
6FC5398-4DP10-0BA6, 09/2017
9.3
Correcting a part program
As soon as a syntax error in the part program is detected by the control system, program execution is interrupted and the
syntax error is displayed in the alarm line. In this case, you can correct the error directly in the machining operating area with
the program correction function. When making program changes, the control system must be brought into the reset state.
Note
The program correction function is not available for program execution from external.
Operating sequence
Prerequisite: A part program is loaded in "AUTO" mode in the machining operating area.
1.
Press this key on the MCP to place the program in the reset mode.
2.
Press this softkey to activate the block editing window.
3.
Make the necessary corrections. Any changes to the program will be stored immediately.
4.
After you finish the program correction, press this softkey to switch back to the block display
window.
5.
Press this key on the MCP to restart the machining of the program.
9.4
Simultaneous recording during machining of the workpiece
You can follow machining of the workpiece on the screen while the program is being executed on the machine.
Operating sequence
1.
Select the program management operating area.
2.
Enter the target program directory and position the cursor on the desired program.
3.
Press this softkey and the system automatically changes to "AUTO" mode in the machining
operating area.
4.
Press this softkey to open the simultaneous recording window.
5.
Press this key to start the recording. The machining of the workpiece is started and graph-
ically displayed on the screen.
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
49
9.5
Entering the tool wear offsets
Note
You must distinguish the direction of tool wear compensation clearly.
Two methods are available for entering the tool wear offsets: absolute input and incremental input (default: absolute input).
Operating sequence for absolute input
1.
Select the offset operating area.
2.
Open the tool wear window.
3.
Use the cursor keys to select the required tools and their edges.
4.
Enter the desired tool length wear parameter and the tool radius wear parameter (range of
value in mm: -9.999 to 9.999).
Positive value: the tool compensates in a direction of moving away from the workpiece.
Negative value: the tool compensates in a direction of approaching the workpiece.
Note:
If there is already a non-zero offset value in the input field (for example, the existing tool
length offset value is "0.1") and you desire to increase the offset value, then you can either
directly enter the sum of the existing offset value and the increment, or call the pocket calcu-
lator to work out the tool wear offset (proceed through Steps 6 to 9).
5.
Press this key or move the cursor to activate the compensation.
6.
If you desire to use the pocket calculator, position the cursor on the desired input field and
press this key. Then the pocket calculator is opened:
Programming and Operating Manual (Milling)
50
6FC5398-4DP10-0BA6, 09/2017
7.
Enter the desired arithmetic statement in the input line of the pocket calculator.
8.
Press this key and the calculation result is displayed in the pocket calculator:
9.
Press this softkey to enter the result in the input field at the current cursor position and close
the pocket calculator automatically.
Note:
For more information about how to use the pocket calculator, see Section "Pocket calculator
(Page 77)".
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
51
Operating sequence for incremental input
1.
Select the offset operating area.
2.
Open the tool wear window.
3.
Position the cursor bar on the input field to be modified.
4.
Switch to incremental input.
5.
Enter the desired increment value, for example, 0.1.
•
Positive value: the tool compensates in a direction of moving away from the workpiece.
•
Negative value: the tool compensates in a direction of approaching the workpiece.
Note:
Alternatively, you can call the pocket calculator to work out the increment value (see Steps
7 to 10).
6.
Press this key or move the cursor to activate the compensation. Then the value displayed in
the input field becomes the sum of the original value and the increment value.
7.
If you desire to use the pocket calculator, press this key.
Programming and Operating Manual (Milling)
52
6FC5398-4DP10-0BA6, 09/2017
8.
Enter the desired arithmetic statement in the input line of the pocket calculator.
9.
Press this key and the calculation result (for example, 0.1) is displayed in the pocket calcu-
lator:
10.
Press this softkey to add the calculation result to the value in the input field at the current
cursor position and close the pocket calculator automatically.
Note:
For more information about how to use the pocket calculator, see Section "Pocket calculator
(Page 77)".
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
53
10
Other common operations
10.1
Program control functions
You can perform further program control operations through the following operation:
+
→
10.1.1
Program test
With this softkey activated, the part program is executed with no axis or spindle movement. In this
way, you can check the programmed axis positions and auxiliary function outputs of a part program.
This softkey functions the same as the following key on the MCP:
10.1.2
Dry run feedrate
With this softkey activated, all traversing motions are performed with the dry run feedrate defined in
SD42100 DRY_RUN_FEED. You can set the dry run feedrate in the JOG data setting window
through the following operation:
+
→
10.1.3
Conditional stop
With this softkey activated, the processing of the program stops at the end of every block containing
M01. In this way, you can check the result already obtained during the machining of a workpiece.
This softkey functions the same as the following key on the MCP:
Note that in order to continue executing the program, press the following key again:
10.1.4
Skip block
It is possible to skip program blocks, which are not to be executed every time the program runs.
With this softkey activated, the program blocks identified with a slash in front of the block number
(e.g. "/N100") are skipped during machining. Several consecutive blocks can be skipped.
10.1.5
Single block mode
With this softkey activated, the system can interrupt the machining of the workpiece after each
program block. In this way, you can control the machining result block-by-block and check individu-
al machining steps. This softkey functions the same as the following key on the MCP:
The program is advanced to the next block via the following key:
However, for the thread blocks (G33), a stop is performed at the end of the current thread block
only with dry run feedrate activated.
Programming and Operating Manual (Milling)
54
6FC5398-4DP10-0BA6, 09/2017
10.1.6
Rapid traverse override
With this softkey activated, the traversing speed of the axes in the rapid traverse mode (G00) can
be controlled via the feedrate override switch on the MCP.
This softkey functions the same as the following key on the MCP:
It is recommended that you keep this function activated for easy feedrate control during machining.
10.1.7
Auxiliary function lock
With this softkey activated, the part program is executed with the spindle disabled and all auxiliary
functions (see below) suppressed.
Auxiliary function
Address
Tool selection
T
Tool offset
D, DL
Feedrate
F
Spindle speed
S
M functions
M
H functions
H
10.2
Calibrating the tool probe
Preconditions
● The machine manufacturer must have connected the probe to the control system. For more information, see the
SINUMERIK 808D/SINUMERIK 808D ADVANCED Function Manual.
● You must first enter the radius or diameter of the tool for probe calibration.
Operating sequences
Setting the probe data
1.
Select the machining operating area.
2.
Switch to "JOG" mode.
3.
Open the lower-level menu for tool measurement.
4.
Open the auto tool measurement window.
5.
Press this vertical softkey to open the probe data setting window, which shows the coordi-
nates of the probe. Enter the values in the input fields as required (see table below for the
parameter descriptions). See the machine coordinate system for all position values.
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
55
①
Absolute position of the probe in Z direction
②/③
The measured probe center (the machine coordinate)
④
The diameter of the probe (the measured value will be shown after calibrating)
⑤
The thickness of the probe
⑥
The measurement feedrate in "JOG" mode (this parameter is used to create the measuring program)
⑦
G17, G18 and G19 for selection
⑧
Spindle speed in r.p.m.
⑨
Direction of rotation of the spindle: M3, M4, or M5
⑩
Safety distance between the measuring surface of the probe and the tool
Calibrating the probe
1.
Select the machining operating area.
2.
Switch to "JOG" mode.
3.
Open the lower-level menu for tool measurement.
4.
Open the auto tool measurement window.
5.
Press this vertical softkey to enter the probe calibration screen.
6.
You can use this vertical softkey to choose whether to calibrate the tool length and diame-
ter, or to calibrate the tool length only.
7.
Move the tool until it presses down on the measuring surface of the probe. Then the calibra-
tion process is triggered automatically.
Note:
When calibrating the probe, make sure the tool is approximately aligned with the center of
the measuring surface of the probe.
During the automatic measurement, a dial gauge symbol (
) displays, which indicates
that the measuring process is active.
Programming and Operating Manual (Milling)
56
6FC5398-4DP10-0BA6, 09/2017
10.3
Measuring the tool with a probe (auto)
Preconditions
● The machine manufacturer must parameterize special measuring functions for tool probe measuring. For more
information, see the SINUMERIK 808D/SINUMERIK 808D ADVANCED Function Manual.
● You must first enter the cutting edge position and calibrate the probe (Page 54) before the actual measurement.
Operating sequence
1.
Select the machining operating area.
2.
Switch to "JOG" mode.
3.
Open the lower-level menu for tool measurement.
4.
Open the auto tool measurement window. The tool length in the Z direction is measured by
default.
5.
Move the tool until it presses down on the edge of the probe. Then the tool length is calcu-
lated and entered in the tool list. Note that if several axes move simultaneously, no offset
data can be calculated.
6.
Press this vertical softkey to measure the tool diameter in the X and Y planes.
7.
Move the tool until it presses down on the edge of the probe. The tool diameter or radius is
calculated and entered in the tool list. Note that if several axes move simultaneously, no
offset data can be calculated.
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
57
10.4
Setting up the workpiece
10.4.1
Measuring the workpiece
Overview
You must select the relevant offset panel (for example, G54) and the axis you want to determine for the offset first.
Before measuring, you can start the spindle by following the steps in Section "Activating the tool and the spindle (Page 23)".
Operating sequence
Workpiece edge measurement
1.
Select the machining operating area.
2.
Switch to "JOG" mode.
3.
Open the window for workpiece measurement.
4.
Press this vertical softkey to open the window for measurement at the workpiece edge.
5.
Press this softkey to measure in the X direction.
6.
Traverse the tool, which has been measured previously, to approach the workpiece in the X
direction.
7.
Switch to handwheel control mode.
8.
Select a suitable override feedrate, and then use the handwheel to move the tool to scratch
the required workpiece edge.
Programming and Operating Manual (Milling)
58
6FC5398-4DP10-0BA6, 09/2017
9.
Select the offset plane to save in and the measuring direction (for example, "G54" and "-").
10.
Enter the distance (for example, "0") in the following window.
Press this key or move the cursor to confirm your input.
11.
Press this vertical softkey. The workpiece offset of the X axis is calculated automatically and
displayed in the offset field.
12.
Repeat the above operations to measure and set the workpiece offsets in axes Y and Z
respectively.
Rectangular workpiece measurement
1.
Select the machining operating area.
2.
Switch to "JOG" mode.
3.
Open the lower-level menu for workpiece measurement.
4.
Open the window for measurement of a rectangular workpiece.
5.
Traverse the tool, which has been measured previously, in the direction of the orange arrow
P1 shown in the measuring window, in order to scratch the workpiece edge with the tool tip.
6.
Press this softkey to save the tool position P1 in the coordinate system. To cancel the rec-
ord, press the softkey again.
7.
Repeat Steps 5 and 6 to save the other three positions: P2, P3 and P4.
8.
Save the workpiece offsets in axes X and Y after measuring all four positions.
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
59
Circular workpiece measurement
1.
Select the machining operating area.
2.
Switch to "JOG" mode.
3.
Open the lower-level menu for workpiece measurement.
4.
Open the window for measurement of a circular workpiece.
5.
Traverse the tool, which has been measured previously, in the direction of the orange arrow
P1 shown in the measuring window, in order to scratch the workpiece edge with the tool tip.
6.
Press the softkey to save the tool position P1 in the coordinate system. To cancel the rec-
ord, press the softkey again.
7.
Repeat Steps 5 and 6 to save the other two positions: P2 and P3.
8.
Save the workpiece offsets in axes X and Y after measuring all three positions.
10.4.2
Entering/modifying workpiece offsets
Operating sequence
In case of any problems found when testing the tool offset result, you can proceed through the following steps to make tiny
adjustment of values:
1.
Select the offset operating area.
2.
Open the list of workpiece offsets. The list contains the values of the basic offset of the
programmed workpiece offset and the active scaling factors, the mirror status display and
the total of all active workpiece offsets.
Programming and Operating Manual (Milling)
60
6FC5398-4DP10-0BA6, 09/2017
3.
Use the cursor keys to position the cursor bar in the input fields to be modified and enter the
values.
4.
Confirm your entries. The changes to the workpiece offsets are activated immediately.
10.5
Entering/modifying the setting data
Entering/modifying the setting data
Operating sequence
1.
Select the offset operating area.
2.
Open the setting data window.
3.
Open the window for setting the general data.
4.
Position the cursor bar in the input fields to be modified and enter the values (see table
below for the parameter descriptions).
5.
Use this key or move the cursor to confirm your entries.
Parameters in the setting data window
①/②
A limitation of the spindle speed in the maximum (G26)/minimum (G25) fields can only be performed within the
limit values defined in the machine data.
③
For thread cutting, a start position for the spindle is displayed as the start angle. A multiple thread can be cut by
changing the angle when the thread cutting operation is repeated.
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
61
Setting the time counter
Operating sequence
1.
Select the offset operating area.
2.
Open the setting data window.
3.
Open the time counter window.
4.
Position the cursor bar in the input fields to be modified and enter the values (see table
below for the parameter descriptions).
5.
Use this key or move the cursor to confirm your entries.
Parameters in the window for timers and workpiece counters
①
The total number of workpieces produced (total actual)
②
The number of workpieces required (workpiece setpoint)
③
The number of all workpieces produced since the starting time
④
The total run time of NC programs in "AUTO" mode and the run time of all programs between NC start and end of
program/RESET. The timer is set to zero with each power-up of the control system.
⑤
The run time of the selected NC program in seconds
The default value is 0 each time a new NC program starts up. You can set MD27860 to ensure that this value will be
deleted even if there is a jump to the beginning of the program with GOTOs or in the event of ASUPs (used for tool
change in "JOG" and "MM+" modes) and PROG_EVENTs starting.
⑥
Processing time in seconds
⑦
The time since the last system power-up with default values ("cold restart") in minutes
⑧
The time since the last normal system power-up ("warm restart") in minutes
Note
The timer is automatically reset to zero in case of a control power-up with default values.
Programming and Operating Manual (Milling)
62
6FC5398-4DP10-0BA6, 09/2017
Setting the working area limitation
Operating sequence
1.
Select the offset operating area.
2.
Open the setting data window.
3.
Open the working area limitation window.
4.
Position the cursor on the input field to be modified and enter the required value.
5.
Position the cursor on the checkbox for value activation located after the input field.
6.
Press this key to activate or deactivate your input in Step 4.
Parameters in the window for working area limitation
①
Displays the axes that exist in the machine coordinate system (MCS), workpiece coordinate system (WCS), or
relative coordinate system (REL)
②/④
The minimum/maximum traversing distance specified for the axes
③/⑤
Activates or deactivates the entered minimum/maximum value
⑥
Unit for the traversing distance
Modifying miscellaneous setting data
Operating sequence
+
1.
Select the system data operating area.
2.
Open the window for machine data.
3.
Open the window for the expert list.
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
63
4.
Select a group of setting data you desire to modify.
5.
Press these softkeys to search for your desired setting data with the data number/name.
Alternatively, you can position the cursor on the input field to be modified and enter the
desired value.
To switch to the desired axis when modifying the axis-specific setting data, press the corre-
sponding softkey:
6.
Press this key or move the cursor to confirm your entries.
10.6
Setting R parameters
Functionality
The "R variables" start screen lists the R parameters that exist within the control system. You can set or query these global
parameters in any program as required.
Operating sequence
1.
Select the offset operating area.
2.
Open the list of R parameters.
3.
Press the cursor keys to navigate in the list, and enter the values in the input fields to be
modified.
Note:
You can search for your desired R variable with this softkey. By default, the function
searches the R number.
You can press this softkey to activate the option of searching by R name. Define the R
name as desired, if necessary.
4.
Press this key or move the cursor to confirm your entries.
For more information about R parameters, see Section "Arithmetic parameter R (Page 126)".
Programming and Operating Manual (Milling)
64
6FC5398-4DP10-0BA6, 09/2017
10.7
Setting user data
Functionality
The "User data" start screen lists the user data that exist within the control system. You can set or query these global
parameters in any program as required.
Operating sequence
1.
Select the offset operating area.
2.
Open the list of user data.
3.
Use the cursor keys to navigate in the list, and enter the values in the input fields to be mod-
ified.
Note:
You can search for your desired user data with this softkey.
You can press this softkey to continue searching your desired user data.
4.
Use this key or move the cursor to confirm your entries.
10.8
Setting the date and time
By default, the system date and time remain the factory settings. You can proceed through the following operating sequence
to change the date and time as required.
Operating sequence
+
1.
Select the system data operating area.
2.
Open the date and time setting window through the following softkey operations:
→
3.
Enter the date and time in the specified format.
4.
Press this softkey to confirm your settings.
Note
The settings of date and time are effective for 30 days if the control system is powered off for a long time at 25 °C
surrounding air temperature.
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
65
10.9
Configuring the operating area after startup
The machining operating area is displayed by default after the startup of the control system. Alternatively, you can select
another operating area which you desire to enter after the system starts up.
Operating sequence
+
1.
Select the system data operating area.
2.
Open the window for setting the startup operating area through the following softkey opera-
tions:
→
3.
Use the cursor keys to select the desired operating area in the following window:
4.
Press this softkey to confirm your setting, and the configured operating system will display
after the control system restarts.
10.10
Executing/transferring a part program from external
Note
You're recommended to use the Notepad editor with ANSI character encoding to create/edit part program files on the
computer. Program files in other encoding formats (for example, Unicode) may cause unexpected errors after being
imported into the control system.
10.10.1
Executing/transferring through the USB interface
The USB interface on the front of the PPU can be used to connect to a USB device, for example:
● An external USB memory stick, to transfer data between the USB stick and the control system
● An external USB keyboard which functions as an external NC keyboard
Programming and Operating Manual (Milling)
66
6FC5398-4DP10-0BA6, 09/2017
10.10.1.1 Executing from external (through USB interface)
Prerequisite: A USB memory stick (which includes the part program to be executed) is inserted in the front USB interface of
the PPU.
Proceed as follows to execute a part program from external through the USB interface:
1.
Select the program management operating area.
2.
Press this softkey to enter the USB directory, and select the program file you desire to exe-
cute.
3.
To directly execute the program, press this softkey. The system automatically switches to
"AUTO" mode in the machining operating area. The program is transferred to the buffer
memory on the control system and then displayed in the following window:
You can also press this key on the PPU to view the program blocks first before executing.
Then press the following softkey to execute:
4.
If desired, you can use this softkey to specify how you want the program to be executed.
For more information of the program control, refer to Section "Program control functions
(Page 53)" .
5.
Press this key to execute the program. The program is reloaded continuously.
Either at the end of the program or after pressing this key, the program is automatically
removed from the control system.
Note
The USB directory is automatically identified if a USB stick is inserted.
Do not remove the USB stick during the external program execution through the USB interface.
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
67
10.10.1.2 Transferring from external (through USB interface)
Prerequisite: A USB memory stick (which includes the part program to be transferred) is inserted in the front USB interface
of the PPU.
Proceed as follows to transfer a part program from external through the USB interface:
1.
Select the program management operating area.
2.
Press this softkey to enter the USB directory.
3.
Select the program file you desire to transfer.
4.
Press this softkey to copy the file to the buffer memory on the control system.
5.
Enter the program directory.
6.
Press this softkey to paste the copied file into the program directory.
10.10.2
Executing/transferring through the Ethernet connection
10.10.2.1 Configuring the network drive
A connected network drive allows you to access a shared directory on your computer from the control system. The network
drive functions based on the Ethernet connection between the control system and a computer. The following Ethernet
connections are possible:
● Direct connection: connecting the control system directly to a computer
● Network connection: integrating the control system into an existing Ethernet network
Establishing a direct connection
Proceed as follows to establish a direct connection:
1.
Connect the control system with the computer using an Ethernet cable.
+
2.
Select the system data operating area.
3.
Press the extension key.
4.
Enter the main screen of the service control options through the following softkey opera-
tions:
→
5.
Press this softkey to set up a direct connection between the control system and the com-
puter.
The following dialog box pops up on the screen:
Programming and Operating Manual (Milling)
68
6FC5398-4DP10-0BA6, 09/2017
Establishing a network connection
Proceed as follows to establish a network connection:
1.
Connect the control system with the local network using an Ethernet cable.
+
2.
Select the system data operating area on the PPU.
3.
Press the extension key.
4.
Enter the main screen of the service control options through the following softkey opera-
tions:
→
5.
Press this softkey to enter the window for the network configuration.
Note: make sure this vertical softkey is not selected.
6.
Configure the network as required in the following window:
You can configure the DHCP with this key.
Note: if you select "No" for DHCP, you must enter the IP address (which must belong to the
same network as that of your computer) and subnet mask manually.
7.
Press this softkey to save the configuration. If you select "Yes" for DHCP, you also need to
restart the control system to activate the network configuration.
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
69
Creating and connecting a network drive
Proceed as follows to create and connect a network drive:
1.
Share a directory on your local disk on your computer.
2.
Select the program management operating area.
3.
Press this softkey to go to the network drive directory.
4.
Press this softkey to go to the window for configuring the network drives.
5.
Press this key to select a drive identifier: N1, N2, or N3.
6.
Move the cursor to the following input fields:
①: Enter the user name of your Windows account
②: Enter the logon password (case sensitive) of your Windows account
③: Enter the IP address of the server and the share name of the shared directory on your
computer. Example: //140.231.196.90/808D
7.
Press this softkey to confirm and the configured network drive appears on the screen as
follows. The drive icon is yellow if the network drive is connected successfully; otherwise,
the icon is gray.
You can delete a selected network drive using this softkey.
Note
After you properly configure all the settings for the direct connection between the control system and the network drive, if the
network drive connection is still invalid, contact your Windows system administrator for possible problems with your
operating system configuration.
Programming and Operating Manual (Milling)
70
6FC5398-4DP10-0BA6, 09/2017
10.10.2.2 Executing from external (through Ethernet connection)
Prerequisites:
● An Ethernet connection has been established between the control system and the computer.
● A network drive (which includes the part program to be executed) has been created and connected.
Proceed as follows to execute a part program from external through the Ethernet connection:
1.
Select the program management operating area.
2.
Press this softkey to view the network drive(s) created.
3.
Select the desired network drive (which includes the part program to be executed) and
press this key to open it.
4.
Select the program file you desire to execute.
5.
Press this softkey and the system automatically switches to "AUTO" mode in the machining
operating area. The program is transferred to the buffer memory on the control system and
then displayed in the following window:
6.
If desired, you can use this softkey to specify how you want the program to be executed.
For more information of the program control, refer to Section "Program control functions
(Page 53)".
7.
Press this key to execute the program. The program is reloaded continuously.
Either at the end of the program or after pressing this key, the program is automatically
removed from the control system.
10.10.2.3 Transferring from external (through Ethernet connection)
Prerequisites:
● An Ethernet connection has been established between the control system and the computer.
● A network drive (which includes the part program to be transferred) has been created and connected.
Proceed as follows to transfer a part program from external through the Ethernet connection:
1.
Select the program management operating area.
2.
Press this softkey to view the network drive(s) created.
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
71
3.
Select the desired network drive (which includes the part program to be transferred) and
press this key to open it.
4.
Select the program file you desire to transfer.
5.
Press this softkey to copy the file to the buffer memory on the control system.
6.
Enter the program directory.
7.
Press this softkey to paste the copied file into the program directory.
10.10.3
Configuring the firewall
Configuring the firewall
Secure access and communication is achieved through the security function of the integrated firewall. You can open the
window for firewall configuration through the following operations:
+
→
→
→
→
Configurable ports are listed in the following window:
The ports are disabled by default and can be enabled when necessary. To change the port status, select the relevant port
using the cursor keys and press either of the following keys to enable or disable the port:
/
Programming and Operating Manual (Milling)
72
6FC5398-4DP10-0BA6, 09/2017
WARNING
Network security risks due to improper firewall configuration
Improper firewall configuration may cause network security risks, for example, data leakage, virus invasion, and hacker
attack. This may lead to incorrect parameterization or machine malfunction, which in turn can result in death, severe
injuries and/or property damage.
•
Do not use the control system inside a network infrastructure without an additional security product.
•
Make sure that you disable the unnecessary ports in the firewall configuration.
Note
After you disable a communication port, the existing connection established earlier via this port will not be disabled until you
manually disconnect it or the control system restarts/powers off. Therefore, it is recommended that you disconnect the
established connections or restart the control system after disabling the ports.
10.11
Extending/deactivating the CNC lock function
To extend/deactivate the CNC lock function, you must import the corresponding activation/deactivation file (.clc format)
provided by the machine manufacturer into the control system. The file can be imported either directly via an Ethernet
connection (network drive) or alternatively via a storage medium (for example, USB memory stick). The control system must
be in the reset state for the import.
Im porting the activation/deactivation file
Proceed through the following steps to import the file:
1.
•
To import the file via USB, store the file in a USB memory stick and insert the USB
memory stick into the USB interface at the front of the PPU.
•
To import the file via Ethernet, store the file in a shared folder (network drive) on your
computer and connect the network drive via Ethernet connection.
+
2.
Select the system data operating area.
3.
Press this key to view the extended softkeys.
4.
Open the license key dialog box through the following softkey operations:
→
→
5.
Press this softkey to open the file opening dialog box.
6.
Select the target directory (USB or network drive) and press this key to open it.
7.
Locate the desired activation/deactivation file and press this softkey to import.
After the file is imported successfully, you can check the CNC lock status on the HMI
screen, for example:
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
73
•
CNC lock function extended (with a new lock date):
•
CNC lock function deactivated (with no lock date):
Note
If an error occurs when importing the activation file, an error-specific alarm will be issued. The state of the CNC lock function
remains unchanged.
Note
We recommend that you create a complete commissioning archive over all control system components after deactivating the
CNC lock function. If necessary, this commissioning archive can be used to recommission the control system without re-
deactivating the CNC lock function.
Faulty settings of date
If a date earlier than the actual date is set for activated CNC lock function, alarm 8065 is issued after NC restart and then NC
start is disabled. In this case, you must correct the date and perform an NC restart again to clear the alarm.
If during the correcting, a future date is set inadvertently, alarm 8066 is issued. Provided no NC restart has been performed,
the date can still be corrected. After NC restart, a date set in the future is considered as being an actual date and can no
longer be reset.
NOTICE
Shorter service life
After NC restart, a future date set earlier than the lock date reduces the service life until the lock date. If a date equal to or
later than the lock date is set, alarm 8064 is issued and the NC start disabled.
Make sure you set the date correctly prior to NC restart.
Programming and Operating Manual (Milling)
74
6FC5398-4DP10-0BA6, 09/2017
10.12
Data backup
10.12.1
Internal data backup
You can save the NC and PLC data of the volatile memory to the permanent memory of the control system.
Note
After changing important data, it is recommended to carry out an internal data backup immediately.
Backing up data internally
Prerequisite:
● A valid system password has been set on the control system.
● There is no program currently being executed.
Proceed through the following steps to save data:
+
1.
Select the system data operating area.
2.
Press this softkey to open the window for data saving.
3.
Press this softkey to start saving. Do not carry out any operator actions while the data back-
up is running.
Loading internally backed up data
There are two methods to load the saved data.
Method 1:
1.
Press this key while the control system is booting.
2.
Use the cursor keys to select "Reload saved user data" in the setup menu.
3.
Press this key to confirm.
Method 2:
+
1.
Select the system data operating area.
2.
Press this softkey.
3.
Enter the NC startup screen.
4.
Use the cursor keys to select the third startup mode as follows:
5.
Press this softkey to confirm. The control system restarts with the saved data.
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
75
Note
The following message is displayed on the screen after the control system starts up successfully with the saved data:
You must enter the password again after you have powered up the control system with the saved data.
10.12.2
External data backup
10.12.2.1 External data backup in a data archive
You can perform a complete data backup of the control system by creating a startup archive.
Backing up data externally in a data archive
+
1.
Select the system data operating area.
2.
Press this softkey to open the window for creating or restoring a startup archive.
There are three options for creating a data archive. Note that options ① and ③ are visible
only with the manufacturer password.
① Creates a data archive for series machine commissioning
② Creates a data archive for a complete system backup
③ Backs up the complete system data on the system CompactFlash Card (CF card)
3.
Select option ② and press this softkey to confirm, and the dialog box for saving the archive
file opens.
The name of the data archive is "arc_startup.arc" by default. You can also use your favorite
name. The file name extension ".arc" must be entered.
4.
Select your desired directory and press this key to open it.
Note that you can press this key on the PPU to toggle between the file name input field and
the directory selection area.
5.
Press this softkey to confirm and the archive information dialog box opens.
6.
Specify the properties of the archive and press this softkey. The control system starts crea-
tion of the startup archive.
Programming and Operating Manual (Milling)
76
6FC5398-4DP10-0BA6, 09/2017
Note
Do not remove the USB stick in the process of data backup if you choose USB as the target directory.
Pressing when you are in any operating area creates a startup archive on the connected USB stick. In addition,
it automatically saves the action log to the USB stick.
Restoring a startup archive
+
1.
Select the system data operating area.
2.
Press this softkey to open the startup archive window.
3.
Select the following option and press this softkey to restore the startup archive:
4.
Select the backup path to locate the archive file and press this softkey to confirm.
5.
Press this softkey to confirm the archive information.
6.
Press this softkey to continue and start restoring the startup archive. The control system
restarts to complete restoring the archive.
10.12.2.2 External data backup of separate files
In the program management operating area, program files or directories can be copied into another directory or onto a
different drive by means of copying and pasting operations.
Operating sequence
1.
Select the program management operating area.
2.
Enter the program directory.
3.
Select the program file or directory to be backed up.
4.
Press this softkey to copy the file to the clipboard.
5.
Select a desired directory or drive as the data target.
Backs up the files in the folder for storing the user cycles on the control system. This folder
is visible with the manufacturer password.
Backs up the files onto a USB stick.
Backs up the files onto a computer. This requires a connected network drive on the control
system. For more information, see section "Configuring the network drive (Page 67)".
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
77
Backs up the files in the folder for storing the manufacturer files on the control system. This
folder is visible with the manufacturer password.
Backs up the files in the folder for storing end user files on the control system.
6.
Press this softkey to paste the copied data into the current directory.
For more information about data backup, refer to the SINUMERIK 808D/SINUMERIK 808D ADVANCED Diagnostics
Manual.
10.13
Pocket calculator
You can activate the calculator function by pressing this key on the PPU when you position the cursor on the
desired input field to calculate the cycle relevant parameters, contour parameters, tool parameters, workpiece
offsets, R parameters, etc.
For calculating, the four basic arithmetic operations are available, as well as the functions "sine", "cosine", "squaring" and
"square root". A bracket function is provided to calculate nested terms. The bracket depth is unlimited.
If the input field is already occupied by a value, the function will accept this value into the input line of the pocket calculator.
Pressing this softkey empties the input line of the calculator.
After inputting a desired arithmetic statement in the input line of the calculator, pressing this key
starts the calculation. The result is displayed in the pocket calculator.
Selecting this softkey enters the result in the input field at the current cursor position and closes the
pocket calculator automatically.
Pressing this softkey aborts the calculation result (if any) and exits the pocket calculator.
Programming and Operating Manual (Milling)
78
6FC5398-4DP10-0BA6, 09/2017
Characters that may be entered
+, -, *, /
Basic arithmetic operations
S
Sine function
The X value (in degrees) in front of the input cursor is replaced by the sin(X) value.
O
Cosine function
The X value (in degrees) in front of the input cursor is replaced by the cos(X) value.
Q
Square function
The X value in front of the input cursor is replaced by the X2 value.
R
Square root function
The X value in front of the input cursor is replaced by the √X value.
( )
Bracket function (X+Y)*Z
Calculation examples
Task
Input -> Result
100 + (67*3)
100+67*3 -> 301
sin(45_)
45 S -> 0.707107
cos(45_)
45 O -> 0.707107
42
4 Q -> 16
√4
4 R -> 2
(34+3*2)*10
(34+3*2)*10 -> 400
To calculate auxiliary points on a contour, the pocket calculator offers the following functions:
● Calculating the tangential transition between a circle sector and a straight line
● Moving a point in the plane
● Converting polar coordinates to Cartesian coordinates
● Adding the second end point of a straight line/straight line contour section given from an angular relation
11
Programming principles
11.1
Fundamentals of programming
11.1.1
Program names
Each program must have a program name. The program name must follow the conventions below:
● Use a maximum of 24 letters or 12 Chinese characters for a program name (the character length of the file extension
excluded)
● Separate the file extension only with a decimal point
● Enter the file extension ".SPF" if the current default program type is MPF (main program) and you desire to create a
subprogram
● Enter the file extension ".MPF" if the current default program type is SPF (subprogram) and you desire to create a main
program
● Do not enter the file extension if you desire to take the current default program type
● Avoid using special characters for program names.
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
79
Example
11.1.2
Program structure
Structure and content
The NC program consists of a sequence of blocks (see the table below). Each block represents a machining step.
Instructions are written in the blocks in the form of words. The last block in the execution sequence contains a special word
for the end of the program, for example, M2.
The following table shows you an example of the NC program structure.
Block
Word
Word
Word
...
; Comment
Block
N10
G0
X20
...
; First block
Block
N20
G2
Z37
...
; Second block
Block
N30
G91
...
...
; ...
Block
N40
...
...
...
Block
N50
M2
; End of program
11.2
Programming instructions
11.2.1
Programming dimensions
In this section you will find descriptions of the commands, with which you can directly program dimensions taken from a
drawing. This has the advantage that no extensive calculations have to be made for NC programming.
Note
The commands described in this section stand in most cases at the start of an NC program. The way, in which these
functions are combined, is not intended to be a patent remedy. For example, the choice of working plane may be made at
another point in the NC program. The real purpose of this and the following sections is to illustrate the conventional structure
of an NC program.
Overview of typical dimensions
The basis of most NC programs is a drawing with concrete dimensions.
When implementing in a NC program, it is helpful to take over exactly the dimensions of a workpiece drawing into the
machining program. These can be:
● Absolute dimension, G90 modally effective applies for all axes in the block, up to revocation by G91 in a following block.
● Absolute dimension, X=AC(value) only this value applies only for the stated axis and is not influenced by G90/G91. This
is possible for all axes and also for SPOS, SPOSA spindle positionings, and interpolation parameters I, J, K.
● Absolute dimension, X=DC(value) directly approaching the position by the shortest route, only this value applies only for
the stated rotary axis and is not influenced by G90/G91. This is also possible for SPOS, SPOSA spindle positionings.
● Absolute dimension, X=ACP(value) approaching the position in positive direction, only this value is set only for the rotary
axis, the range of which is set to 0... < 360 degrees in the machine data.
● Absolute dimension, X=ACN(value) approaching the position in negative direction, only this value is set only for the
rotary axis, the range of which is set to 0... < 360 degrees in the machine data.
● Incremental dimension, G91 modally effective applies for all axes in the block, until it is revoked by G90 in a following
block.
Programming and Operating Manual (Milling)
80
6FC5398-4DP10-0BA6, 09/2017
● Incremental dimension, X=IC(value) only this value applies exclusively for the stated axis and is not influenced by
G90/G91. This is possible for all axes and also for SPOS, SPOSA spindle positionings, and interpolation parameters I, J,
K.
● Inch dimension, G70 applies for all linear axes in the block, until revoked by G71 in a following block.
● Metric dimension, G71 applies for all linear axes in the block, until revoked by G70 in a following block.
● Inch dimension as G70, however, G700 applies also for feedrate and length-related setting data.
● Metric dimension as G71, however, G710 applies also for feedrate and length-related setting data.
● Diameter programming, DIAMON on
● Diameter programming, DIAMOF off
Diameter programming, DIAM90 for traversing blocks with G90. Radius programming for traversing blocks with G91.
11.2.2
Plane selection: G17 to G19
Functionality
To assign, for example, tool radius and tool length compensations, a plane with two axes is selected from the three axes X,
Y and Z. In this plane, you can activate a tool radius compensation.
For drill and cutter, the length compensation (length1) is assigned to the axis standing vertically on the selected plane. It is
also possible to use a 3-dimensional length compensation for special cases.
Another influence of plane selection is described with the appropriate functions (e.g. Section "Support for the contour
definition programming").
The individual planes are also used to define the direction of rotation of the circle for the circular interpolation CW or CCW.
In the plane in which the circle is traversed, the abscissa and the ordinate are designed and thus also the direction of
rotation of the circle. Circles can also be traversed in a plane other than that of the currently active G17 to G19 plane (For
more information, see Section "Circular interpolation (Page 93)".).
The following plane and axis assignments are possible:
G function
Plane (abscissa/ordinate)
Vertical axis on plane
(length compensation axis when drilling/milling)
G17
X/Y
Z
G18
Z/X
Y
G19
Y/Z
X
See the following illustration for planes and axes when drilling/milling:
Programming example
N10 G17 T... D... M...
; X/Y plane selected
N20 ... X... Y... Z...
; tool length compensation (length1) in Z axis
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
81
11.2.3
Absolute/incremental dimensioning: G90, G91, AC, IC
Functionality
With the instructions G90/G91, the written positional data X, Y, Z... are evaluated as a coordinate point (G90) or as an axis
position to traverse to (G91). G90/G91 applies to all axes.
Irrespective of G90/G91, certain positional data can be specified for certain blocks in absolute/incremental dimensions using
AC/IC.
These instructions do not determine the path by which the end points are reached; this is provided by a G group (G0, G1,
G2 and G3.... For more information, see Sections "Linear interpolation (Page 91)" and "Circular interpolation (Page 93)".).
Programming
G90
; Absolute dimension data
G91
; Incremental dimension data
X=AC(...)
; Absolute dimensioning for a certain axis (here: X axis), non-modal
X=IC(...)
; Incremental dimensioning for a certain axis (here: X axis), non-modal
See the following illustration for different dimensioning types in the drawing:
Absolute dimensioning G90
With absolute dimensioning, the dimensioning data refers to the zero of the coordinate system currently active (workpiece or
current workpiece coordinate system or machine coordinate system). This is dependent on which offsets are currently
active: programmable, settable, or no offsets.
Upon program start, G90 is active for all axes and remains active until it is deselected in a subsequent block by G91
(incremental dimensioning data) (modally active).
Incremental dimensioning G91
With incremental dimensioning, the numerical value of the path information corresponds to the axis path to be traversed.
The leading sign indicates the traversing direction.
G91 applies to all axes and can be deselected in a subsequent block via G90 (absolute dimensioning).
Specification with =AC(...), =IC(...)
After the end point coordinate, write an equality sign. The value must be specified in round brackets.
Absolute dimensions are also possible for circle center points using =AC(...). Otherwise, the reference point for the circle
center is the circle starting point.
Programming example
N10 G90 X20 Z90
; Absolute dimensions
N20 X75 Z=IC(-32)
; X-dimensions remain absolute, incremental Z dimension
N180 G91 X40 Z20
; Switch-over to incremental dimensioning
N190 X-12 Z=AC(17)
; X-remains incremental dimensioning, Z-absolute
Programming and Operating Manual (Milling)
82
6FC5398-4DP10-0BA6, 09/2017
11.2.4
Dimensions in metric units and inches: G71, G70, G710, G700
Functionality
If workpiece dimensions that deviate from the base system settings of the control system are present (inch or mm), the
dimensions can be entered directly in the program. The required conversion into the base system is performed by the control
system.
Programming
G70
; Inch dimensions
G71
' Metric dimensions
G700
; Inch dimensions, also for feedrate F
G710
; Metric dimensions, also for feedrate F
Programming example
N10 G70 X10 Z30
; Inch dimensions
N20 X40 Z50
;G70 continues to act
N80 G71 X19 Z17.3
; metric dimensioning from this point on
Information
Depending on the default setting you have selected, the control system interprets all geometric values as either metric or
inch dimensions. Tool offsets and settable work offsets including their display are also to be understood as geometrical
values; this also applies to the feedrate F in mm/min or inch/min. The default setting can be set via machine data.
All examples listed in this manual are based on a m etric default setting.
G70 or G71 evaluates all geometric parameters that directly refer to the workpiece, either as inches or metric units, for
example:
● Positional data X, Y, Z, ... for G0,G1,G2,G3,G33, CIP, CT
● Interpolation parameters I, J, K (also thread pitch)
● Circle radius CR
● Programmable work offset (TRANS, ATRANS)
● Polar radius RP
All remaining geometric parameters that are not direct workpiece parameters, such as feedrates, tool offsets, and settable
work offsets, are not affected by G70/G71.
G700/G710 however, also affects the feedrate F (inch/min, inch/rev. or mm/min, mm/rev.).
11.2.5
Polar coordinates, pole definition: G110, G111, G112
Functionality
In addition to the common specification in Cartesian coordinates (X, Y, Z), the points of a workpiece can be specified using
the polar coordinates.
Polar coordinates are also helpful if a workpiece or a part of it is dimensioned from a central point (pole) with specification of
the radius and the angle.
Plane
The polar coordinates refer to the plane activated with G17 to G19. In addition, the third axis standing vertically on this plane
can be specified. When doing so, spatial specifications can be programmed as cylinder coordinates.
Polar radius RP=...
The polar radius specifies the distance of the point to the pole. It is stored and must only be written in blocks in which it
changes, after changing the pole or when switching the plane.
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
83
Polar angle AP=...
The angle is always referred to the horizontal axis (abscissa) of the plane (for example, with G17: X axis). Positive or
negative angle specifications are possible.
The polar angle remains stored and must only be written in blocks in which it changes, after changing the pole or when
switching the plane.
See the following illustration for polar radius and polar angle with definition of the positive direction in different planes:
Pole definition, programming
G110
Pole specification relative to the setpoint position last programmed (in the plane, e.g. with G17: X/Y)
G111
; Pole specification relative to the origin of the current workpiece coordinate system (in the plane, e.g. with
G17: X/Y)
G112
; Pole specification, relative to the last valid pole; preserve plane
Note
Pole specifications
•
Pole definitions can also be performed using polar coordinates. This makes sense if a pole already exists.
•
If no pole is defined, the origin of the current workpiece coordinate system will act as the pole.
Programming example
N10 G17
; X/Y plane
N20 G0 X0 Y0
N30 G111 X20 Y10
; Pole coordinates in the current workpiece coordinate system
N40 G1 RP=50 AP=30 F1000
N50 G110 X-10 Y20
N60 G1 RP=30 AP=45 F1000
N70 G112 X40 Y20
; New pole, relative to the last pole as a polar coordinate
N80 G1 RP=30 AP=135
; Polar coordinate
M30
Traversing with polar coordinates
The positions programmed using polar coordinates can also be traversed as positions specified with Cartesian coordinates
as follows:
● G0 - linear interpolation with rapid traverse
● G1 - linear interpolation with feedrate
● G2 - circular interpolation CW
● G3 - circular interpolation CCW
(See also Sections "Linear interpolation (Page 91)" and "Circular interpolation (Page 93)".)
Programming and Operating Manual (Milling)
84
6FC5398-4DP10-0BA6, 09/2017
11.2.6
Programmable work offset: TRANS, ATRANS
Functionality
The programmable work offset can be used:
● for recurring shapes/arrangements in various positions on the workpiece
● when selecting a new reference point for the dimensioning
● as a stock allowance when roughing
This results in the current workpiece coordinate system. The rewritten dimensions use this as a reference.
The offset is possible in all axes.
Programming
TRANS X... Y... Z...
; programmable offset, deletes old instructions for offsetting, rotation, scaling factor,
mirroring
ATRANS X... Y... Z...
; programmable offset, additive to existing instructions
TRANS
; without values: clears old instructions for offset, rotation, scaling factor, mirroring
The instructions which contain TRANS or ATRANS each require a separate block.
See the following illustration for the example for programmable offset:
Programming example
N20 TRANS X20 Y15
; Programmable offset
N30 L10
; Subroutine call; contains the geometry to be offset
N70 TRANS
; Offset cleared
Subroutine call - see Section "Subroutine technique (Page 132)".
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
85
11.2.7
Programmable rotation: ROT, AROT
Functionality
The rotation is performed in the current plane G17 or G18 or G19 using the value of RPL=... specified in degrees.
Programming
ROT RPL=...
; Programmable rotation, deletes old instructions for offsetting, rotation, scaling factor, mirroring
AROT RPL=...
; Programmable rotation, additive to existing instructions
ROT
; Without values: clears old instructions for offset, rotation, scaling factor, mirroring
The instructions which contain ROT or AROT each require a separate block.
See the following illustration for definition of the positive direction of the angle of rotation in the individual planes:
See the following illustration for programming example for programmable offset and rotation:
Programming example
N10 G17 ...
; X/Y plane
N20 TRANS X20 Y10
; Programmable offset
N30 L10
; Subroutine call; contains the geometry to be offset
N40 TRANS X30 Y26
; New offset
N50 AROT RPL=45
; Additive 45 degree rotation
N60 L10
; Subroutine call
N70 TRANS
; Offset and rotation cleared
Subroutine call - see Section "Subroutine technique (Page 132)".
Programming and Operating Manual (Milling)
86
6FC5398-4DP10-0BA6, 09/2017
11.2.8
Programmable scale factor: SCALE, ASCALE
Functionality
A scale factor can be programmed for all axes with SCALE/ASCALE. The path is enlarged or reduced by this factor in the
axis specified. The currently set coordinate system is used as the reference for the scale change.
Programming
SCALE X... Y... Z...
; Programmable scaling factor, clears the old instructions for offset, rotation, scaling factor,
mirroring
ASCALE X... Y... Z...
; Programmable scaling factor, additive to existing instructions
SCALE
; Without values: clears the old instructions for offset, rotation, scaling factor, mirroring
The instructions which contain SCALE or ASCALE each require a separate block.
Note
For circles, the same factor should be used in both axes.
If ATRANS is programmed with SCALE/ASCALE active, these offset values are also scaled.
See the following illustration for example for scaling and offset:
Programming example
N10 G17
; X/Y plane
N20 L10
; Programmed contour original
N30 SCALE X2 Y2
; Contour in X and Y enlarged two times
N40 L10
N50 ATRANS X2.5 Y18
; Offset values are also scaled
N60 L10
Subroutine call - see Section "Subroutine technique (Page 132)".
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
87
11.2.9
Programmable mirroring: MIRROR, AMIRROR
Functionality
MIRROR and AMIRROR can be used to mirror workpiece shapes on coordinate axes. All traversing motions of axes for
which mirroring is programmed are reversed in their direction.
Programming
MIRROR X0 Y0 Z0
; Programmable mirroring, clears old instructions for offset, rotation, scaling factor,
mirroring
AMIRROR X0 Y0 Z0
; Programmable mirroring, additive to existing instructions
MIRROR
; Without values: clears old instructions for offset, rotation, scaling factor, mirroring
The instructions that contain MIRROR or AMIRROR each require a separate block. The axis value has no influence. A
value, however, must be specified.
Note
Any active tool radius compensation (G41/G42) is reversed automatically when mirroring.
The direction of rotation of the circle G2/G3 is also reversed automatically when mirroring.
See the following illustration for example for mirroring with the tool position shown:
Programming example
Mirroring in different coordinate axes with influence on an active tool radius compensation and G2/G3:
...
N10 G17
; X/Y plane, Z standing vertically on it
N20 L10
; Programmed contour with G41
N30 MIRROR X0
; Direction changed in X
N40 L10
; Mirrored contour
N50 MIRROR Y0
; Direction changed in Y
N60 L10
N70 AMIRROR X0
; Mirroring once more, but now in X
N80 L10
; Twice-mirrored contour
N90 MIRROR
; Mirroring off
Subroutine call - see Section "Subroutine technique (Page 132)".
Programming and Operating Manual (Milling)
88
6FC5398-4DP10-0BA6, 09/2017
11.2.10
Workpiece coordinate system - settable work offset: G54 to G59, G500, G53,
G153
Functionality
The settable work offset specifies the position of the workpiece zero on the machine (offset of the workpiece zero with
respect to the machine zero). This offset is determined upon clamping of the workpiece into the machine and must be
entered in the corresponding data field by the operator. The value is activated by the program by selection from six possible
groupings: G54 to G59.
Note
Workpiece clamping at an angle is possible by entering the angles of rotation around the machine axes. These rotation
portions are activated with the work offset G54 to G59.
Programming
G54 to G59
; 1. to 6th settable work offset
G500
; Settable work offset OFF - modal
G53
; settable work offset OFF, non-modal, also suppresses programmable offset
G153
;settable work offset OFF, non-modal; additionally suppresses base frame
See the following illustration for settable work offset:
See the following illustration for various workpiece clamping positions when drilling/milling:
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
89
Programming example
N10 G54
; Call first settable work offset
N20 L47
; Machining of workpiece 1, here using L47
N30 G55
; Call second settable work offset
N40 L47
; Machining of workpiece 2, here using L47
N50 G56
; Call third settable work offset
N60 L47
; Machining of workpiece 3, here using L47
N70 G57
; Call fourth settable work offset
N80 L47
; Machining of workpiece 4, here using L47
N90 G500 G0 X
; Deactivate settable work offset
Subroutine call - see Section "Subroutine technique (Page 132)".
11.2.11
NC block compression (COMPON, COMPCURV, COMPCAD)
Functionality
CAD/CAM systems normally produce linear blocks, which meet the configured accuracy specifications. In the case of
complex contours, a large volume of data and short path sections can result. The short path sections restrict the processing
rate.
By using a compressor function, the contour, specified by using linear blocks, is approached using polynomial blocks. This
has the following advantages:
● Reduction of the number of required part program blocks for describing the workpiece contour
● Continuous block transitions
● Higher maximum path velocities
The following compressor functions are available:
● COMPON
The block transitions are only constant in the velocity, while acceleration of the participating axes can be in jumps at
block transitions.
● COMPCURV
Block transitions have continuous acceleration. This ensures both smooth velocity and acceleration of all axes at block
transitions.
● COMPCAD
The compression that uses a lot of computation time and memory space is optimized regarding surface quality and
speed. COMPCAD should only be used if measures to improve the surface cannot be taken by the CAD/CAM program in
advance.
COMPOF terminates the compressor function.
Syntax
COMPON
COMPCURV
COMPCAD
COMPOF
Meaning
COMPON:
Command to activate the compressor function COMPON.
Effective:
Modal
COMPCURV:
Command to activate the compressor function COMPCURV.
Effective:
Modal
COMPCAD:
Command to activate the compressor function COMPCAD.
Effective:
Modal
COMPOF :
Command to deactivate the currently active compressor function.
Programming and Operating Manual (Milling)
90
6FC5398-4DP10-0BA6, 09/2017
Supplementary conditions
● The NC block compression is generally executed for linear blocks (G1).
● Only blocks that comply with a simple syntax are compressed:
N... G1X... Y... Z... F... ;comment
All other blocks are executed unchanged (no compression).
● Motion blocks with extended addresses such as C=100 or A=AC(100) are also condensed.
● The position values do not have to be programmed directly, but can also be indirectly specified using parameter
assignments, e.g. X=R1*(R2+R3).
● If the option "orientation transformation" is available, then NC blocks in which the tool orientation (and where relevant,
also the tool rotation) is programmed using direction vectors can also be compressed.
● It is interrupted by any other type of NC instruction, e.g., an auxiliary function output.
Examples
Example 1: COMPON
Program code
Comment
N10 COMPON
; Compressor function COMPON on.
N11 G1 X0.37 Y2.9 F600
; G1 before end point and feed.
N12 X16.87 Y-.698
N13 X16.865 Y-.72
N14 X16.91 Y-.799
…
N1037 COMPOF
; Compressor function off.
…
Example 2: COMPCAD
Program code
Comment
G00 X30 Y6 Z40
G1 F10000 G642
; Blending function G642 on.
SOFT
; Jerk limiting SOFT on.
COMPCAD
; Compressor function COMPCAD on.
STOPFIFO
N24050 Z32.499
N24051 X41.365 Z32.500
N24052 X43.115 Z32.497
N24053 X43.365 Z32.477
N24054 X43.556 Z32.449
N24055 X43.818 Z32.387
N24056 X44.076 Z32.300
…
COMPOF
; Compressor function off.
G00 Z50
M30
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
91
11.3
Linear interpolation
11.3.1
Linear interpolation with rapid traverse: G0
Functionality
The rapid traverse movement G0 is used for rapid positioning of the tool, but not for direct workpiece machining.
All the axes can be traversed simultaneously - on a straight path.
For each axis, the maximum speed (rapid traverse) is defined in machine data. If only one axis traverses, it uses its rapid
traverse. If two or three axes are traversed simultaneously, the path velocity (e.g. the resulting velocity at the tool tip) must
be selected such that the m aximum possible path velocity with consideration of all axes involved results.
A programmed feedrate (F word) has no meaning for G0. G0 remains active until canceled by another instruction from this G
group (G1, G2, G3...).
Programming
G0 X... Y... Z...
; Cartesian coordinates
G0 AP=... RP=...
; Polar coordinates
G0 AP=... RP=... Z...
; Cylindrical coordinates (3-dimensional)
Note
Another option for linear programming is available with the angle specification ANG=... (For more information, see Section
"Contour definition programming (Page 110)".).
See the illustration for linear interpolation with rapid traverse from point P1 to P2:
Programming example
N10 G0 X100 Y150 Z65
; Cartesian coordinate
...
N50 G0 RP=16.78 AP=45
; Polar coordinate
Information
Another group of G functions exists for movement to the position (see Section "Exact stop/continuous-path control mode:
G9, G60, G64 (Page 106)").
For G60 exact stop, a window with various precision values can be selected with another G group. For exact stop, an
alternative instruction with non-modal effectiveness exists: G9.
You should consider these options for adaptation to your positioning tasks.
Programming and Operating Manual (Milling)
92
6FC5398-4DP10-0BA6, 09/2017
11.3.2
Feedrate F
Functionality
The feed F is the path velocity and represents the value of the geometric sum of the velocity components of all axes
involved. The individual axis velocities therefore result from the portion of the axis path in the overall distance to be
traversed.
The feedrate F is effective for the interpolation types G1, G2, G3, CIP, and CT and is retained until a new F word is written.
Programming
F...
Note
For integer values, the decimal point is not required, e.g. F300.
Unit of measure for F with G94, G95
The dimension unit for the F word is determined by G functions:
● G94: F as the feedrate in m m/min
● G95: Feedrate F in mm/spindle revolutions
(only meaningful when the spindle is running)
Note
This unit of measure applies to metric dimensions. According to Section "Metric and inch dimensioning", settings with
inch dimensioning are also possible.
Programming example
N10 G94 F310
; Feedrate in mm/min
N110 S200 M3
; Spindle rotation
N120 G95 F15.5
; Feedrate in mm/revolution
Note
Write a new F word if you change G94 - G95.
11.3.3
Linear interpolation with feedrate: G1
Functionality
The tool moves from the starting point to the end point along a straight path. The path velocity is determined by the
programmed F word.
All axes can be traversed simultaneously.
G1 remains active until canceled by another instruction from this G group (G0, G2, G3...).
Programming
G1 X... Y... Z... F...
; Cartesian coordinates
G1 AP=... RP=... F...
; Polar coordinates
G1 AP=... RP=... Z... F...
; cylindrical coordinates (3-dimensional)
Note
Another option for linear programming is available with the angle specification ANG=... (see Section "Contour definition
programming (Page 110)").
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
93
See the illustration for linear interpolation in three axes using the example of a slot:
Programming example
N05 G0 G90 X40 Y48 Z2 S500 M3
; The tool traverses in rapid traverse on P1,
three axes concurrently, spindle speed = 500 rpm,
clockwise
N10 G1 Z-12 F100
; Infeed on Z-12, feed 100 mm/min
N15 X20 Y18 Z-10
; Tool travels on a straight line in space on P2
N20 G0 Z100
; Retraction in rapid traverse
N25 X-20 Y80
N30 M2
; End of program
To machine a workpiece, spindle speed S ... and direction M3/M4 are required (see Section "Spindle movements
(Page 109)").
11.4
Circular interpolation
11.4.1
Circular interpolation: G2, G3
Functionality
The tool moves from the starting point to the end point along a circular path. The direction is determined by the G function:
G2: clockwise
G3: counter-clockwise
Programming and Operating Manual (Milling)
94
6FC5398-4DP10-0BA6, 09/2017
The description of the desired circle can be given in various ways:
See the following illustration for possibilities of circle programming with G2/G3 using the example of the axes X/Y and G2:
G2/G3 remains active until canceled by another instruction from this G group (G0, G1, ...).
The path velocity is determined by the programmed F word.
Programming
G2/G3 X... Y... I... J...
; End point and center point
G2/G3 CR=... X... Y...
; Circle radius and end point
G2/G3 AR=... I... J...
; Opening angle and center point
G2/G3 AR=... X... Y...
; Opening angle and end point
G2/G3 AP=... RP=...
; Polar coordinates, circle around the pole
Note
Other circle programming instructions:
•
CT - circle with tangential connection
•
CIP - circle via intermediate point (see following sections)
Input tolerances for the circle
Circles are only accepted by the control system with a certain dimensional tolerance. The circle radius at the starting and
end points are compared here. If the difference is within the tolerance, the center point is exactly set internally. Otherwise,
an alarm message is issued.
Information
Full circles in a block are only possible if the center point and the end point are specified.
For circles with radius specification, the arithmetic sign of CR=... is used to select the correct circle. It is possible to program
two circles with the same starting and end points, as well as with the same radius and the same direction. The negative sign
in front of CR=-... determines the circle whose circle segment is greater than a semi-circle; otherwise, the circle with the
circle segment is less than or equal to the semi-circle and determined as follows:
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
95
See the following illustration for selection of the circle from two possible circles with radius specification:
Programming example: Definition of center point and end point
N5 G90 X30 Y40
; Starting point circle for N10
N10 G2 X50 Y40 I10 J-7
; End point and center point
Note
Center point values refer to the circle starting point!
Programming and Operating Manual (Milling)
96
6FC5398-4DP10-0BA6, 09/2017
Programming example: End point and radius specification
N5 G90 X30 Y40
; Starting point circle for N10
N10 G2 X50 Y40 CR=12.207
; End point and radius
Note
With a negative leading sign for the value with CR=-..., a circular segment larger than a semi-circle is selected.
Programming example: Definition of end point and aperture angle
N5 G90 X30 Y40
; Starting point circle for N10
N10 G2 X50 Y40 AR=105
; End point and aperture angle
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
97
Programming example: Definition of center point and aperture angle
N5 G90 X30 Y40
; Starting point circle for N10
N10 G2 I10 J-7 AR=105
; Center point and aperture angle
Note
Center point values refer to the circle starting point!
Programming example: Polar coordinates
N1 G17
; X/Y plane
N5 G90 G0 X30 Y40
; Starting point circle for N10
N10 G111 X40 Y33
; Pole = circle center
N20 G2 RP=12.207 AP=21
; Polar specifications
Programming and Operating Manual (Milling)
98
6FC5398-4DP10-0BA6, 09/2017
11.4.2
Circular interpolation via intermediate point: CIP
Functionality
If you know three contour points of the circle, instead of center point or radius or aperture angle, then it is advantageous to
use the CIP function.
The direction of the circle results here from the position of the intermediate point (between starting and end points). The
intermediate point is written according to the following axis assignment:
I1=... for the X axis,
J1=... for the Y axis,
K1=... for the Z axis.
CIP remains active until canceled by another instruction from this G group (G0, G1, G2, ...).
Note
The configured dimensional data G90 or G91 applies to the end point and the intermediate point.
See the following illustration for circle with end point and intermediate point specification using the example of G90:
Programming example
N5 G90 X30 Y40
;Starting point circle for N10
N10 CIP X50 Y40 I1=40 J1=45
; End point and intermediate point
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
99
11.4.3
Circle with tangential transition: CT
Functionality
With CT and the programmed end point in the current plane G17 through G19, a circle is generated which is connected
tangentially to the previous path segment (circle or straight line) in this plane.
This defines the radius and center point of the circle from the geometric relationships of the previous path section and the
programmed circle end point.
See the following illustration for circle with tangential transition to the previous path section:
Programming example
N10 G1 X20 F300
; Straight line
N20 CT X... Y...
; Circle with tangential connection
11.4.4
Helix interpolation: G2/G3, TURN
Functionality
With helix interpolation, two movements are overlaid:
● Circular movement in the G17, G18 or G19 plane
● Linear movement of the axis standing vertically on this plane.
The number of additional full-circle passes is programmed with TURN=. These are added to the actual circle
programming.
The helix interpolation can preferably be used for the milling of threads or of lubricating grooves in cylinders.
Programming
G2/G3 X... Y... I... J... TURN=...
; Center and end points
G2/G3 CR=... X... Y... TURN=...
; Circle radius and end point
G2/G3 AR=... I... J... TURN=...
; Opening angle and center point
G2/G3 AR=... X... Y... TURN=...
; Opening angle and end point
G2/G3 AP=... RP=... TURN=...
; Polar coordinates, circle around the pole
Programming and Operating Manual (Milling)
100
6FC5398-4DP10-0BA6, 09/2017
See the following illustration for helical interpolation:
Programming example
N10 G17
; X/Y plane, Z standing vertically on it
N20 G0 Z50
N30 G1 X0 Y50 F300
; Approach starting point
N40 G3 X0 Y0 Z33 I0 J-25 TURN= 3
; Helix
M30
11.4.5
Feedrate override for circles: CFTCP, CFC
Functionality
For activated tool radius compensation (G41/G42) and circle programming, it is imperative to correct the feedrate at the
cutter center point if the programmed F value is to act at the circle contour.
Internal and external machining of a circle and the current tool radius are taken into account automatically if the tool radius
compensation is enabled.
This feedrate correction (override) is not necessary for linear paths. The path velocities at the cutter center point and at the
programmed contour are identical.
If you wish the programmed feedrate always to act at the cutter center point path, then disable the feedrate override. The
modally acting G group that contains CFTCP/CFC (G functions) is provided for switching.
Programming
CFTCP
; Feedrate override OFF (the programmed feedrate acts at the milling cutter center point)
CFC
; Feedrate override with circle ON
