Page 1
CNC
8055 ·TC·
Operating manual
Ref.1711
Soft: V02.2x
Page 2
This product uses the following source code, subject to the terms of the GPL license. The applications busybox V0.60.2;
dosfstools V2.9; linux-ftpd V0.17; ppp V2.4.0; utelnet V0.1.1. The librarygrx V2.4.4. The linux kernel V2.4.4. The linux boot
ppcboot V1.1.3. If you would like to have a CD copy of this source code sent to you, send 10 Euros to Fagor Automation
for shipping and handling.
All rights reserved. No part of this documentation may be transmitted,
transcribed, stored in a backup device or translated into another language
without Fagor Automation’s consent. Unauthorized copying or distributing of this
software is prohibited.
The information described in this manual may be subject to changes due to
technical modifications. Fagor Automation reserves the right to change the
contents of this manual without prior notice.
All the trade marks appearing in the manual belong to the corresponding owners.
The use of these marks by third parties for their own purpose could violate the
rights of the owners.
It is possible that CNC can execute more functions than those described in its
associated documentation; however, Fagor Automation does not guarantee the
validity of those applications. Therefore, except under the express permission
from Fagor Automation, any CNC application that is not described in the
documentation must be considered as "impossible". In any case, Fagor
Automation shall not be held responsible for any personal injuries or physical
damage caused or suffered by the CNC if it is used in any way other than as
explained in the related documentation.
The content of this manual and its validity for the product described here has been
verified. Even so, involuntary errors are possible, hence no absolute match is
guaranteed. However, the contents of this document are regularly checked and
updated implementing the necessary corrections in a later edition. We appreciate
your suggestions for improvement.
The examples described in this manual are for learning purposes. Before using
them in industrial applications, they must be properly adapted making sure that
the safety regulations are fully met.
DUAL-USE PRODUCTS
Products manufactured by FAGOR AUTOMATION since April 1st 2014 will
include "-MDU" in their identification if they are included on the list of dual-use
products according to regulation UE 428/2009 and require an export license
depending on destination.
Page 3
Operating manual
CNC 8055
CNC 8055i
SOFT: V02.2X
·3·
INDEX
About the product ......................................................................................................................... 7
Declaration of conformity and Warranty conditions ...................................................................... 9
Version history ............................................................................................................................ 11
Safety conditions ........................................................................................................................ 15
Returning conditions ................................................................................................................... 19
Additional notes .......................................................................................................................... 21
Fagor documentation.................................................................................................................. 23
CHAPTER 1 GENERAL CONCEPTS
1.1 Keyboard........................................................................................................................ 25
1.2 General concepts........................................................................................................... 27
1.2.1 P999997 text program management.......................................................................... 29
1.3 Power-up........................................................................................................................ 30
1.4 Working in T mode with the TC keyboard...................................................................... 31
1.5 Video off......................................................................................................................... 31
1.6 Managing the CYCLE START key................................................................................. 31
CHAPTER 2 OPERATING IN JOG MODE
2.1 Introduction .................................................................................................................... 34
2.1.1 Standard screen of the TC mode ............................................................................... 34
2.1.2 Description of the special screen of the TC mode ..................................................... 36
2.1.3 Selecting a program for simulation or execution ........................................................ 38
2.2 Axis control .................................................................................................................... 39
2.2.1 Work units .................................................................................................................. 39
2.2.2 Coordinate preset....................................................................................................... 39
2.2.3 Managing the axis feedrate (F) .................................................................................. 39
2.3 Machine reference (home) search ................................................................................. 40
2.4 Zero offset table ............................................................................................................. 41
2.5 Jog movement ............................................................................................................... 42
2.5.1 Moving an axis to a particular position (coordinate)................................................... 42
2.5.2 Incremental movement............................................................................................... 42
2.5.3 Continuous jog ........................................................................................................... 43
2.5.4 Path-jog...................................................................................................................... 44
2.5.5 Movement with an electronic handwheel ................................................................... 46
2.5.6 Feed handwheel......................................................................................................... 47
2.5.7 Path-handwheel ......................................................................................................... 48
2.6 Tool control .................................................................................................................... 49
2.6.1 Tool change ............................................................................................................... 50
2.6.2 Variable tool change point.......................................................................................... 51
2.7 Tool calibration............................................................................................................... 52
2.7.1 Define the tool in the tool table (level 1)..................................................................... 53
2.7.2 Manual tool calibration with/without a probe (level 1) ................................................ 56
2.7.3 Tool calibration with a probe (level 2) ........................................................................ 58
2.7.4 Probe calibration (level 3) .......................................................................................... 60
2.7.5 Manual tool calibration without stopping the spindle .................................................. 61
2.8 Live tool.......................................................................................................................... 62
2.9 Spindle control ............................................................................................................... 64
2.9.1 Spindle in rpm ............................................................................................................ 65
2.9.2 Spindle in constant surface speed mode ................................................................... 67
2.9.3 Spindle orientation ..................................................................................................... 69
2.10 Controlling the external devices..................................................................................... 71
2.11 ISO management........................................................................................................... 72
CHAPTER 3 WORKING WITH OPERATIONS OR CYCLES
3.1 Operation editing mode.................................................................................................. 77
3.1.1 Definition of spindle conditions................................................................................... 78
3.1.2 Definition of machining conditions.............................................................................. 79
3.1.3 Cycle level.................................................................................................................. 81
3.2 Simulating and executing the operation......................................................................... 82
3.2.1 Background cycle editing ........................................................................................... 83
3.3 Positioning cycle ............................................................................................................84
3.3.1 Definition of data ........................................................................................................ 85
Page 4
·4·
Operating manual
CNC 8055
CNC 8055i
SOFT: V02.2X
3.4 Turning cycle ................................................................................................................. 86
3.4.1 Data definition (levels 1 and 2) .................................................................................. 89
3.4.2 Data definition (levels 3, 4 and 5) .............................................................................. 91
3.4.3 Basic operation (levels 1 and 2)................................................................................. 93
3.5 Facing cycle................................................................................................................... 95
3.5.1 Data definition (levels 1 and 2) .................................................................................. 98
3.5.2 Data definition (levels 3, 4 and 5) .............................................................................. 99
3.5.3 Basic operation (levels 1 and 2)............................................................................... 101
3.6 Taper turning cycle ...................................................................................................... 103
3.6.1 Definition of data ...................................................................................................... 104
3.6.2 Basic operation ........................................................................................................ 107
3.7 Rounding cycle ............................................................................................................ 109
3.7.1 Geometry definition.................................................................................................. 110
3.7.2 Basic operation ........................................................................................................ 113
3.8 Threading cycle ........................................................................................................... 115
3.8.1 Geometry definition.................................................................................................. 118
3.8.2 Standard threads ..................................................................................................... 124
3.8.3 Basic operation. Longitudinal threading................................................................... 132
3.8.4 Basic operation. Taper threading............................................................................. 133
3.8.5 Basic operation. Face threading .............................................................................. 134
3.8.6 Basic operation. Thread repair................................................................................. 135
3.9 Grooving cycle ............................................................................................................. 136
3.9.1 Calibration of the grooving tool ................................................................................ 138
3.9.2 Geometry definition.................................................................................................. 139
3.9.3 Basic operation. Grooving........................................................................................ 143
3.9.4 Basic operation. Cut off............................................................................................ 145
3.10 Drilling and tapping cycles ........................................................................................... 146
3.10.1 Geometry definition.................................................................................................. 148
3.10.2 Drilling cycle. Basic operation .................................................................................. 150
3.10.3 Tapping cycle. Basic operation ................................................................................ 151
3.10.4 Multiple drilling cycle. Basic operation ..................................................................... 152
3.10.5 Multiple threading cycle. Basic operation................................................................. 153
3.10.6 Multiple slot milling cycle. Basic operation............................................................... 154
3.11 Profiling cycle............................................................................................................... 155
3.11.1 Level 1. Profile definition.......................................................................................... 156
3.11.2 Levels 2, 3 and 4. Profile definition .......................................................................... 158
3.11.3 Level 2. Optimizing of the machining of a profile ..................................................... 159
3.11.4 Definition of geometry levels 1 and 2. ZX profile ..................................................... 160
3.11.5 Definition of geometry at levels 3 and 4. XC, ZC profiles ........................................ 163
3.11.6 Basic operation at levels 1 and 2. ZX profile............................................................ 164
3.11.7 Basic operation at levels 3 and 4. XC, ZC profiles................................................... 165
3.11.8 Example. Level 1 ..................................................................................................... 166
3.11.9 Examples. Level 2.................................................................................................... 167
CHAPTER 4 Y AXIS
4.1 Profiling cycles with Y axis........................................................................................... 177
4.2 Graphics: XY and ZY plane selection .......................................................................... 177
4.3 Tool calibration ............................................................................................................ 178
CHAPTER 5 OPERATING IN ISO MODE
5.1 Editing blocks in ISO mode.......................................................................................... 182
5.2 Programming assistance ............................................................................................. 183
5.2.1 Zero offsets and presets .......................................................................................... 183
5.2.2 Work zones .............................................................................................................. 183
5.2.3 Insert labels and repetitions from label to label........................................................ 183
5.2.4 Mirror image............................................................................................................. 184
5.2.5 Scaling factor ........................................................................................................... 184
Page 5
Operating manual
CNC 8055
CNC 8055i
SOFT: V02.2X
·5·
CHAPTER 6 SAVING PROGRAMS
6.1 List of saved programs................................................................................................. 186
6.2 See the contents of a program..................................................................................... 187
6.2.1 Seeing one of the operations in detail...................................................................... 187
6.3 Edit a new part-program .............................................................................................. 188
6.4 Saving an ISO block or a cycle .................................................................................... 189
6.5 Delete a new part program .......................................................................................... 190
6.6 Copying a part-program into another one .................................................................... 191
6.7 Modify a part-program.................................................................................................. 192
6.7.1 Delete an operation.................................................................................................. 192
6.7.2 Add or insert a new operation .................................................................................. 192
6.7.3 Move an operation to another position..................................................................... 193
6.7.4 Modify an existing operation .................................................................................... 194
6.8 Managing programs using the explorer ....................................................................... 195
CHAPTER 7 EXECUTION AND SIMULATION
7.1 Simulating or executing an operation or cycle ............................................................. 198
7.2 Simulating or executing a part-program....................................................................... 199
7.2.1 Simulating or executing a portion of a part-program ................................................ 199
7.3 Simulating or executing an operation that has been saved ......................................... 200
7.4 Execution mode ........................................................................................................... 201
7.4.1 Tool inspection ......................................................................................................... 202
7.5 Graphic representation ................................................................................................ 203
Page 6
·6·
Operating manual
CNC 8055
CNC 8055i
SOFT: V02.2X
Page 7
CNC 8055
CNC 8055i
·7·
ABOUT THE PRODUCT
BASIC CHARACTERISTICS OF THE DIFFERENT MODELS.
HARDWARE OPTIONS OF THE 8055I CNC
8055i FL EN 8055 FL
8055i FL
8055 Power
8055i Power
Pendant 8055i FL EN 8055i FL 8055i Power
Enclosure ----- 8055 FL 8055 Power
USB Standard Standard Standard
Block processing time 1 ms 3.5 ms 1 ms
RAM memory 1Mb 1Mb 1 Mb
Software for 7 axes ----- ----- Option
TCP transformation ----- ----- Option
C axis (Lathe) ----- ----- Option
Y axis (Lathe) ----- ----- Option
Look-ahead 100 blocks 100 blocks 200 blocks
Flash Memory 512Mb / 2Gb 512Mb Option Option
Analog Digital Engraving
Ethernet Option Option Option
RS232 serial line. Standard Standard Standard
16 digital inputs and 8 outputs (I1 to I16 and O1 to O8) Standard Standard Standard
Another 40 digital inputs and 24 outputs (I65 to I104 and O33 to O56) Option Option Option
Probe inputs Standard Standard Standard
Spindle (feedback input and analog output) Standard Standard Standard
Electronic handwheels Standard Standard Standard
4 axes (feedback and velocity command) Option Option - - -
Remote CAN modules, for digital I/O expansion (RIO). Option Option - - -
Sercos servo drive system for Fagor servo drive connection. - - - Option - - -
CAN servo drive system for Fagor servo drive connection. - - - Option - - -
Before start-up, verify that the machine that integrates this CNC meets the 89/392/CEE Directive.
Page 8
·8·
CNC 8055
CNC 8055i
About the product
SOFTWARE OPTIONS OF THE 8055 AND 8055I CNCS.
Model
GP M MC MCO EN T TC TCO
Number of axes with standard software 4 4 4 4 3 2 2 2
Number of axes with optional software 7 7 7 7 ----- 4 or 7 4 or 7 4 or 7
Electronic threading ----- Stand. Stand. Stand. Stand. Stand. Stand. Stand.
Tool magazine management: ----- Stand. Stand. Stand. ----- Stand. Stand. Stand.
Machining canned cycles ----- Stand. Stand. ----- Stand. Stand. Stand. -----
Multiple machining ----- Stand. Stand. ----- Stand. ----- ----- -----
Solid graphics ----- Stand. Stand. Stand. ----- Stand. Stand. Stand.
Rigid tapping ----- Stand. Stand. Stand. Stand. Stand. Stand. Stand.
Tool life monitoring ----- Opt. Opt. Opt. Stand. Opt. Opt. Opt.
Probing canned cycles ----- Opt. Opt. Opt. Stand. Opt. Opt. Opt.
DNC Stand. Stand. Stand. Stand. Stand. Stand. Stand. Stand.
COCOM version Opt. Opt. Opt. Opt. ----- Opt. Opt. Opt.
Profile editor Stand. Stand. Stand. Stand. ----- Stand. Stand. Stand.
Tool radius compensation Stand. Stand. Stand. Stand. Stand. Stand. Stand. Stand.
Tangential control Opt. Opt. Opt. Opt. ----- Opt. Opt. Opt.
Retracing ----- Opt. Opt. Opt. Stand. Opt. Opt. Opt.
Setup assistance Stand. Stand. Stand. Stand. Stand. Stand. Stand. Stand.
Irregular pockets with islands ----- Stand. Stand. Stand. ----- ----- ----- -----
TCP transformation ----- Opt. Opt. Opt. ----- ----- ----- -----
C axis (on Lathe) ----- ----- ----- ----- ----- Opt. Opt. Opt.
Y axis (on Lathe) ----- ----- ----- ----- ----- Opt. Opt. Opt.
Telediagnosis Opt. Opt. Opt. Opt. Stand. Opt. Opt. Opt.
Page 9
CNC 8055
CNC 8055i
·9·
DECLARATION OF CONFORMITY AND
WARRANTY CONDITIONS
DECLARATION OF CONFORMITY
The declaration of conformity for the CNC is available in the downloads section of FAGOR’S corporate
website at http://www.fagorautomation.com. (Type of file: Declaration of conformity).
WARRANTY TERMS
The warranty conditions for the CNC are available in the downloads section of FAGOR’s corporate website
at http://www.fagorautomation.com. (Type of file: General sales-warranty conditions).
Page 10
·10·
CNC 8055
CNC 8055i
Declaration of conformity and Warranty conditions
Page 11
CNC 8055
CNC 8055i
·11·
VERSION HISTORY
Here is a list of the features added in each software version and the manuals that describe them.
The version history uses the following abbreviations:
INST Installation manual
PRG Programming manual
OPT Operating manual
OPT-MC Operating manual for the MC option.
OPT-TC Operating manual for the TC option.
OPT-CO Manual of the CO manual
Software V01.00 October 2010
First version.
Software V01.20 April 2011
Software V01.08 August 2011
Software V01.30 September 2011
List of features Manual
Open communication. INST
Improvements to Look Ahead machining. INST
Blocks with helical interpolation in G51. PRG
G84. Tapping with relief. PRG
List of features Manual
Spindle parameter OPLDECTI (P86). INST
List of features Manual
Gear ratio management on Sercos spindles INST
Improved feedrate limit management (FLIMIT). INST
New type of penetration in lathe type threading cycles. PRG
Improved lathe type thread repair. Partial repair. PRG
MC option: Rigid tapping with relief. OPT-MC
TC option: New type of penetration in threading cycles. OPT-TC
TC option: Improved thread repair. Partial and multi-entry (start) thread repair. OPT-TC
TC option: Zig-zag entry to the groove at the starting point of the groove. OPT-TC
Page 12
·12·
CNC 8055
CNC 8055i
Version history
Software V01.31 October 2011
Software V01.40 January 2012
Software V01.60 December 2013
Software V01.65 January 2015
Software V02.00 February 2014
List of features Manual
CNC 8055 FL Engraving model INST / OPT/ PRG
List of features Manual
Execution of M3, M4 and M5 using PLC marks INST / PRG
Values 12 and 43 of variable OPMODE in conversational work mode. INST / PRG
List of features Manual
Auto-adjustment of axis machine parameter DERGAIN. INST
New value for axis machine parameter ACFGAIN (P46). INST
Value 120 of the OPMODE variable. INST / PRG
List of features Manual
Block processing time of 1 ms on the "CNC 8055i FL Engraving" model. INST / OPT/ PRG
List of features Manual
Profile machining in segments. J parameter for G66 and G68 cycles. PRG
Calls to subroutines using G functions. INST / PRG
Anticipated tool management. INST
Managing "PNG" and "JPG" graphic elements. INST
New values for parameters MAXGEAR1..4 (P2..5), SLIMIT (P66) and MAXSPEED (P0). INST
Retracing function of 2000 blocks. INST
Quick block search. OPT
Local subroutines within a program. PRG
Avoid spindle stop with M30 or RESET. Spindle parameter SPDLSTOP (P87). INST
Programming T and M06 with associated with a subroutine in the same line. PRG
New values of the OPMODE variable. INST / PRG
New variables: DISABMOD, GGSN, GGSO, GGSP, GGSQ, CYCCHORDERR. INST / PRG
Possibility to set the parameters of SERCOS nodes in a non-sequential order. INST
WRITE instruction: “$” character followed by “P”. PRG
Cancel additive handwheel offset with G04 K0. General parameter ADIMPG (P176). INST / PRG
Ethernet parameter NFSPROTO (P32). TCP or UDP protocol selection. INST
Face thread repair cycle. OPT TC
Penetration increment (step) in thread repair. INST / OPT TC
API compliant thread. OPT TC
Roughing by segments in inside profiling cycles 1 and 2. INST / OPT TC
Programming the Z increment and the angle on threads. INST / OPT TC
Reversal of the starting and final point of the face thread repair. INST / OPT TC
Manual tool calibration without stopping the spindle during each step. INST / OPT TC
Page 13
CNC 8055
CNC 8055i
·13·
Version history
Software V02.03 July 2014
Software V02.10 November 2014
Software V02.21 July 2015
Software V02.22 March 2016
List of features Manual
Set PAGE and SYMBOL instructions support PNG and JPG/JPEG formats. PRG
New values for parameters MAXGEAR1..4 (P2..5), SLIMIT (P66), MAXSPEED (P0) and
DFORMAT (P1).
INST
List of features Manual
Incremental zero offset (G158). INST / PRG
Programs identified with letters. OPT
Variables PRGN and EXECLEV. INST
Korean language. INST
Change of default value for general machine para meters: MAINOFFS (P107), MAINTASF (P162)
and FEEDTYPE (P170).
INST
New variable EXTORG. INST / PRG
Image handling via DNC. PRG
Save/restore a trace of the oscilloscope. OPT
List of features Manual
PLC library. INST
Zero offsets table in ISO mode. OPT
Compensation of the elastic deformation in the coupling of an axis. INST
Machine axis parameter DYNDEFRQ (P103). INST
Change of maximum value of axis and spindle parameter NPULSES. INST
Operating Terms. OPT
List of features Manual
Axis filters for movements with the handwheel. General machine parameter HDIFFBAC (P129)
and machine axis parameter HANFREQ (P104).
INST
Change of maximum value of axis and spindle parameter NPULSES. INST
Page 14
·14·
CNC 8055
CNC 8055i
Version history
Page 15
CNC 8055
CNC 8055i
·15·
SAFETY CONDITIONS
Read the following safety measures in order to prevent harming people or damage to this product and those
products connected to it.
The unit can only be repaired by personnel authorized by Fagor Automation.
Fagor Automation shall not be held responsible of any physical or material damage originated from not
complying with these basic safety rules.
PRECAUTIONS AGAINST PERSONAL HARM
• Interconnection of modules.
Use the connection cables provided with the unit.
• Use proper Mains AC power cables
To avoid risks, use only the Mains AC cables recommended for this unit.
• Avoid electric shocks.
In order to avoid electrical discharges and fire hazards, do not apply electrical voltage outside the range
selected on the rear panel of the central unit.
• Ground connection.
In order to avoid electrical discharges, connect the ground terminals of all the modules to the main
ground terminal. Before connecting the inputs and outputs of this unit, make sure that all the grounding
connections are properly made.
• Before powering the unit up, make sure that it is connected to ground.
In order to avoid electrical discharges, make sure that all the grounding connections are properly made.
• Do not work in humid environments.
In order to avoid electrical discharges, always work under 90% of relative humidity (non-condensing)
and 45 ºC (113º F).
• Do not operate this unit in explosive environments.
In order to avoid risks, harm or damages, do not work in explosive environments.
Page 16
·16·
CNC 8055
CNC 8055i
Safety conditions
PRECAUTIONS AGAINST PRODUCT DAMAGE
• Work environment.
This unit is ready to be used in industrial environments complying with the directives and regulations
effective in the European Community.
Fagor Automation shall not be held responsible for any damage that could suffer or cause when installed
under other conditions (residential or domestic environments).
• Install this unit in the proper place.
It is recommended, whenever possible, to install the CNC away from coolants, chemical product, blows,
etc. that could damage it.
This unit meets the European directives on electromagnetic compatibility. Nevertheless, it is
recommended to keep it away from sources of electromagnetic disturbance, such as:
Powerful loads connected to the same mains as the unit.
Nearby portable transmitters (radio-telephones, Ham radio transmitters).
Nearby radio / TC transmitters.
Nearby arc welding machines.
Nearby high voltage lines.
Etc.
•Enclosures.
It is up to the manufacturer to guarantee that the enclosure where the unit has been installed meets
all the relevant directives of the European Union.
• Avoid disturbances coming from the machine tool.
The machine-tool must have all the interference generating elements (relay coils, contactors, motors,
etc.) uncoupled.
DC relay coils. Diode type 1N4000.
AC relay coils. RC connected as close to the coils as possible with approximate values of R=220
1 W y C=0,2 µF / 600 V.
AC motors. RC connected between phases, with values of R=300 / 6 W y C=0,47 µF / 600 V.
• Use the proper power supply.
Use an external regulated 24 Vdc power supply for the inputs and outputs.
• Connecting the power supply to ground.
The zero Volt point of the external power supply must be connected to the main ground point of the
machine.
• Analog inputs and outputs connection.
It is recommended to connect them using shielded cables and connecting their shields (mesh) to the
corresponding pin.
• Ambient conditions.
The working temperature must be between +5 ºC and +40 ºC (41ºF and 104º F)
The storage temperature must be between -25 ºC and +70 ºC. (-13 ºF and 158 ºF)
• Monitor enclosure (CNC 8055) or central unit ( CNC 8055i)
Guarantee the required gaps between the monitor or the central unit and each wall of the enclosure.
Use a DC fan to improve enclosure ventilation.
• Power switch.
This power switch must be mounted in such a way that it is easily accessed and at a distance between
0.7 meters (27.5 inches) and 1.7 meters (5.5ft) off the floor.
Page 17
CNC 8055
CNC 8055i
·17·
Safety conditions
PROTECTIONS OF THE UNIT ITSELF (8055)
• "Axes" and "Inputs-Outputs" modules.
All the digital inputs and outputs have galvanic isolation via optocouplers between the CNC circuitry
and the outside.
They are protected by an external fast fuse (F) of 3.15 A 250V against overvoltage of the external power
supply (over 33 Vdc) and against reverse connection of the power supply.
• Monitor.
The type of protection fuse depends on the type of monitor. See identification label of the unit itself.
PROTECTIONS OF THE UNIT ITSELF (8055I)
• Central unit.
It has a 4 A 250V external fast fuse (F).
• Inputs-Outputs.
All the digital inputs and outputs have galvanic isolation via optocouplers between the CNC circuitry
and the outside.
OUT
IN
X7
X1
X8
X9
X2
X10
X3
X11X4X12
X5
X13
X6
+24V
0V
FUSIBLE
FUSES
Page 18
·18·
CNC 8055
CNC 8055i
Safety conditions
PRECAUTIONS DURING REPAIRS
SAFETY SYMBOLS
• Symbols that may appear in the manual.
Do not manipulate the inside of the unit. Only personnel authorized by Fagor Automation may access
the interior of this unit.
Do not handle the connectors with the unit connected to AC power. Before manipulating the connectors
(inputs/outputs, feedback, etc.) make sure that the unit is not connected to AC power.
Symbol for danger or prohibition.
It indicates actions or operations that may cause damage to people or to units.
Warning or caution symbol.
It indicates situations that could be caused by certain operations and the actions to take to prevent
them.
Mandatory symbol.
It indicates actions or operations that MUST be carried out.
Information symbol.
It indicates notes, warnings and advises.
i
Page 19
CNC 8055
CNC 8055i
·19·
RETURNING CONDITIONS
When sending the central nit or the remote modules, pack them in its original package and packaging
material. If you do not have the original packaging material, pack it as follows:
1. Get a cardboard box whose 3 inside dimensions are at least 15 cm (6 inches) larger than those of the
unit itself. The cardboard being used to make the box must have a resistance of 170 kg. (375 pounds).
2. Attach a label indicating the owner of the unit, person to contact, type of unit and serial number.
3. In case of failure, also indicate the symptom and a short description of the failure.
4. Protect the unit wrapping it up with a roll of polyethylene or with similar material.
5. When sending the central unit, protect especially the screen.
6. Pad the unit inside the cardboard box with polyurethane foam on all sides.
7. Seal the cardboard box with packaging tape or with industrial staples.
Page 20
·20·
CNC 8055
CNC 8055i
Returning conditions
Page 21
CNC 8055
CNC 8055i
·21·
ADDITIONAL NOTES
Mount the CNC away from coolants, chemical products, blows, etc. which could damage it. Before turning
the unit on, verify that the ground connections have been made properly.
To prevent electrical shock at the central unit of the 8055 CNC, use the proper mains AC connector at the
power supply module. Use 3-wire power cables (one for ground connection).
To prevent electrical shock at the monitor of the 8055 CNC, use the proper mains AC connector (A) with
3-wire power cables (one of them for ground connection).
Before turning on the monitor of the 8055 CNC and verifying that the external AC line (B) fuse of each unit
is the right one. See identification label of the unit itself.
In case of a malfunction or failure, disconnect it and call the technical service. Do not get into the inside
of the unit.
FAGOR
I/O
X1
X2
X3
AXES
X1 X2
X3 X4
X5 X6
X7 X8
X9
X10
CPU
X1 X2
CMPCT
FLASH
ETH
COM1
X3
C
D
E
F
0
B
A
9
8
1
7
2
6
3
5
4
IN
OUT
NODE
USB
(A)
(B)
X1
W1
Page 22
·22·
CNC 8055
CNC 8055i
Additional notes
Page 23
CNC 8055
CNC 8055i
·23·
FAGOR DOCUMENTATION
OEM manual
It is directed to the machine builder or person in charge of installing and starting-up the CNC.
USER-M manual
Directed to the end user.
It describes how to operate and program in M mode.
USER-T manual
Directed to the end user.
It describes how to operate and program in T mode.
MC Manual
Directed to the end user.
It describes how to operate and program in MC mode.
It contains a self-teaching manual.
TC Manual
Directed to the end user.
It describes how to operate and program in TC mode.
It contains a self-teaching manual.
MCO/TCO model
Directed to the end user.
It describes how to operate and program in MCO and TCO mode.
Examples-M manual
Directed to the end user.
It contains programming examples for the M mode.
Examples-T manual
Directed to the end user.
It contains programming examples for the T mode.
WINDNC Manual
It is directed to people using the optional DNC communications software.
It is supplied in a floppy disk with the application.
WINDRAW55 Manual
Directed to people who use the WINDRAW55 to create screens.
It is supplied in a floppy disk with the application.
Page 24
·24·
CNC 8055
CNC 8055i
Fagor documentation
Page 25
CNC 8055
CNC 8055i
·TC· OPTION
SOFT: V02.2X
1
·25·
GENERAL CONCEPTS
1.1 Keyboard
Alphanumeric keyboard and command keys
Specific keys of the TC model
Select the X character.
Select the A character.
Select the R character.
These keys may be used for:
• Selecting and defining the machining operations.
• Govern the external devices.
• Selecting the spindle work mode.
• Selecting the single block or automatic execution Mode.
FAGOR
LEVEL
CYCLE
ZERO
O2 O4
O5O3O1
PCALL
ISO
HELP
i
GRAPHICS
CSS
m / min
SINGLE
ENTER
RECALL
P.PROG
CLEAR
ESC
RESET
C+
C-
+
-
SPINDLE
SPEED
%
100
10
1
100
10
1
1000
10000
JOG
0
2
4
10
20
30
405060
70
80
90
100
110
120
FEED %
EY
Z 4
G(5H)6I$
X
AR7BU8CV9DW
J"
F 1
K'2L;3M:
NÑ
S -
+=00?·PSP
ALT
Q!TSHIFT
]
* /<> [
ENTER
RECALL
P.PROG
CLEAR
ESC
RESET
EY
Z 4G(5H)6
I$
XAR7BU8CV9
DW
J"
F 1K'2L;3
M:
NÑ
S -+=00?·
PSP
ALT
Q!TSHIFT
]
* /<> [
X
AR
SHIFT
X
AR
X
AR
ALT
FAGOR
LEVEL
CYCLE
ZERO
O2 O4
O5O3O1
PCALL
ISO
HELP
i
GRAPHICS
CSS
m / min
SINGLE
Page 26
·26·
Operating manual
CNC 8055
CNC 8055i
1.
GENERAL CONCEPTS
·TC· OPTION
SOFT: V02.2X
Keyboard
JOG keys
These keys may be used for:
• Moving the axes of the machine.
• Governing the spindle.
• Modifying the feedrate of the axes and the spindle speed.
• Starting and stopping the execution.
C+
C-
+
-
SPINDLE
SPEED
%
100
10
1
100
10
1
1000
10000
JOG
0
2
4
10
20
30
405060
70
80
90
100
110
120
FEED %
Page 27
Operating manual
CNC 8055
CNC 8055i
GENERAL CONCEPTS
1.
·TC· OPTION
SOFT: V02.2X
·27·
General concepts
1.2 General concepts
It offers all the features of the T model plus those specific of the TC mode. For example, the CNC
setup must be done in T mode.
In TC work mode, programs P900000 through P999999 are reserved for the CNC itself; in other
words, the user cannot use them as part-programs.
On the other hand, in order to work in TC mode, the CNC must have programs P999997 and
P999998 stored in its memory. Both programs are related to the software version and, consequently,
are not supplied by Fagor Auto mation. Whenever the CNC detects a new software version, it updates
these programs automatically and, for safety, it makes a copy of the old ones in the KeyCF.
Likewise, subroutines 0000 through 8999 are free to use and subroutines 9000 through 9999 are
reserved for the CNC.
Subroutines reserved for the CNC
Some of the subroutines reserved for the CNC have the following meaning:
Both subroutines must be defined by the machine manufacturer, even when no operation is to be
carried out at the beginning and at the end of the part-program. If they are not defined, the CNC
will issue an error message when trying to execute a part-program.
OEM (manufacturer's) parameters
OEM parameters and subroutines with OEM parameters can only be used in OEM programs; those
defined with the [O] attribute. Modifying one of these parameters in the tables requires an OEM
password.
When using OEM parameters in the configuration programs, this program must have the [O]
attribute; otherwise, the CNC will issue an error when editing the user cycles that refer to OEM
parameters in write mode.
Programs P999997 and P999998 are associated with the software version. Fagor Automation shall
not be held responsible of the CNC's performance if programs P999997 and P999998 have been
deleted from memory or do not match the software version.
9998 Subroutine that the CNC will execute at the beginning of each part-program.
9999 Subroutine that the CNC will execute at the end of each part-program.
Every time a new part-program is edited, the CNC inserts a call to the relevant
subroutine at the beginning and at the end of the program.
Example of how to define subroutine 9998.
(SUB 9998) ; Definition of subroutine 9998.
··· ; Program blocks defined by the OEM.
(RET) ; End of subroutine.
Page 28
·28·
Operating manual
CNC 8055
CNC 8055i
1.
GENERAL CONCEPTS
·TC· OPTION
SOFT: V02.2X
General concepts
Programs reserved for the CNC
Some of the programs reserved for the CNC have the following meaning:
P999998
It is a program of subroutines that the CNC uses to interpret the programs edited in TC format and
execute them later on.
P999997
It is a text program that contains:
• The sentences and texts that will be displayed on the various screens of the TC mode.
• The help texts for the icons, in the work cycles, that are shown on the lower left side of the screen.
• The messages (MSG) and errors (ERR) that may come up at the TC model.
All the texts, messages and errors that may be translated into the desired language.
Considerations about the texts
The format of a line is as follows:
;Text number - explanatory comment (not displayed) - $Text to be displayed
All the program lines must begin with the ";" character and the text to be displayed must be preceded
by the "$" symbol. If a line begins with ";;", the CNC assumes that the whole line is a program
comment.
Examples:
;44 $M/MIN Is message 44 and displays the text "M/MIN"
;;General text The CNC treats it as a comment
;;44 Feedrate $M/MIN The CNC treats it as a comment
;44 Feedrate $M/MIN Is message 44 whose hidden explanatory comment is
"Feedrate" and displays the text "M/MIN"
Considerations about the messages
The format must be respected. Only the text after SAVEMSG may be translated:
Example:
Original message: N9500(MSG"SAVEMSG: TURNING CYCLE")
Translated message: N9500(MSG"SAVEMSG: ZILINDRAKETA ZIKLOA")
Considerations about the errors
The format must be respected. Only the text between quote marks ("text") may be translated.
Example:
Original text: N9000(ERROR"Cycle without roughing")
Translated text: N9000(ERROR"Arbastatu gabeko zikloa")
P998000 ··· P998999
They are the profiles defined by the user with the profile editor. In the TC mode, the user defines
them with 3 digits (from 0 to 999) and the CNC saves them internally as P998xxx.
This program must not be modified. If this program is modified or deleted, Fagor Automation will not
be held responsible of the CNC's performance.
If the manufacturer needs to create his own subroutines (for home search, tool change, etc.), as well
as subroutines 9998 and 9999, they must be included in another program, for example P899999.
When modifying program 999997, it is recommended to make a backup copy of it because the CNC
replaces that program when selecting another language or updating the software version.
i
Page 29
Operating manual
CNC 8055
CNC 8055i
GENERAL CONCEPTS
1.
·TC· OPTION
SOFT: V02.2X
·29·
General concepts
1.2.1 P999997 text program management
On power up, the CNC copies the texts of program P999997 into the system memory.
• It checks if program P999997 is in user memory, if not, it looks in the KeyCF and if it is not there
either, it assumes the default ones and copies them into program P999997 of the user memory.
• When selecting mainland Chinese, it ignores program P999997 and it always assumes the
default ones.
If when switching from T mode to TC or TCO mode, it cannot find program P999997 because it has
been deleted, it is initialized like on power-up.
When modifying the texts of program P999997, turn the CNC off and back on so it assumes the
new texts.
The CNC carries out the following operations when changing the language, the software version
and when adding TC, TCO conversational modes (new software features):
• It copies, for safety, the texts that were being used into KeyCF as program P999993.
• It deletes the program P999997 that may be in the KeyCF.
• It assumes the new texts that are provided by default and copies them into program P999997
of the user memory.
To change the texts, after modifying program P999997, turn the CNC off and back on so it assumes
the new texts.
Page 30
·30·
Operating manual
CNC 8055
CNC 8055i
1.
GENERAL CONCEPTS
·TC· OPTION
SOFT: V02.2X
Power-up
1.3 Power-up
The standard screen of the TC mode is the following:
On power-up and after the keystroke sequence [SHIFT] [RESET], the CNC shows
"page 0" defined by the manufacturer; if there is no "page 0", it shows the standard
screen of the work mode. Press any key to access the work mode.
There are 2 work modes: TC work mode and T work mode. To change from one
work mode to another, press the key sequence [SHIFT] [ESC].
SHIFT
RESET
15:28:42 SBK P000002 IN POSITION
X
Z
S
00044.000
-00443.331
0
REFERENCE ZERO X 0000.000
REFERENCE ZERO Z 0000.000
00025.000
00000.013
00014.480
F 0100.000
% 080
T 02
S 0100
D 12
CHANGE POSITION
X 25.000 Z 85.000
% 115
SMAX 1000 RANGE 1
020.0000
ESC
SHIFT
The CNC setup must be done in T mode.
Likewise, some errors must be eliminated in T mode.
Page 31
Operating manual
CNC 8055
CNC 8055i
GENERAL CONCEPTS
1.
·TC· OPTION
SOFT: V02.2X
·31·
Working in T mode with the TC keyboard
1.4 Working in T mode with the TC keyboard
The TC keyboard is designed to also be able to work in T mode. In T mode, use the alphanumeric
keyboard and the keys that replace the softkeys F1 through F7.
1.5 Video off
Also, any message (PLC, program, etc.) restores the CNC image.
1.6 Managing the CYCLE START key
In order to avoid undesired executions when pressing key sequences that are not supported in TC
mode, the CNC changes the "Start" icon at the top of the window from green to gray and shows a
message indicating that it is an invalid action.
For example, if "M3 Start" is pressed (sequence not supported in TC mode) while a part-program
is selected, the CNC issues a warning and prevents the selected part-program from running when
detecting the "Start" key.
There are 2 work modes: TC work mode and T work mode. To change from one
work mode to another, press the key sequence [SHIFT] [ESC].
Alphanumeric keyboard:
The keys that replace the softkeys F1 through F7
are:
ESC
SHIFT
ENTER
RECALL
P.PROG
CLEAR
ESC
RESET
EY
Z 4G(5H)6
I$
XAR7BU8CV9
DW
J"
F 1K'2L;3
M:
NÑ
S -+=00?·
PSP
ALT
Q!TSHIFT
]
* /<> [
F1 F7
The keystroke sequence [SHIFT] [CLEAR] clears the CRT screen (it goes blank).
Press any key to restore the image.
CLEAR
SHIFT
Page 32
·32·
Operating manual
CNC 8055
CNC 8055i
1.
GENERAL CONCEPTS
·TC· OPTION
SOFT: V02.2X
Managing the CYCLE START key
Page 33
CNC 8055
CNC 8055i
·TC· OPTION
SOFT: V02.2X
2
·33·
OPERATING IN JOG MODE
The standard screen of the TC mode is the following:
When pressing the [TWO-COLOR] key, the CNC shows the special screen of the TC mode.
15:28:42 SBK P000002 IN POSITION
X
Z
S
00044.000
-00443.331
0
REFERENCE ZERO X 0000.000
REFERENCE ZERO Z 0000.000
00025.000
00000.013
00014.480
F 0100.000
% 080
T 02
S 0100
D 12
CHANGE PO SITION
X 25.000 Z 85.000
% 115
SMAX 1000 RANGE 1
020.0000
T
15:28:42 SBK P000002 IN POSITION
M0
(MSG " " )
(IF P102 EQ 1 GOTO N10)
(IF P101 EQ 0 RET)
M3
(RET)
N10 M4
(RET)
G01 G18
M41
PARTC : 000000
CYTIME : 00:00:00:00
TIMER: : 000000:00:00
COMMAND
X 00020.000
Z 00089.520
C 00014.480
U 00025.000
THEORETICAL
ACTUAL
X 00020.000
Z 00089.520
C 00014.480
RPM M/MIN
TO GO
X 00000.000
Z 00000.000
C 00000.000
X 00000.000
Z 00000.000
C 00000.000
FOLLOWING ERROR
S 0.0000 S 0.0000 S 0.0000 S 0.0000
B 00000.013
Page 34
·34·
Operating manual
CNC 8055
CNC 8055i
2.
OPERATING IN JOG MODE
·TC· OPTION
SOFT: V02.2X
Introduction
2.1 Introduction
2.1.1 Standard screen of the TC mode
The standard screen of the TC mode offers the following data:
1. Clock.
2. This window may show the following data:
SBK When "single block" execution mode is selected.
DNC When the DNC mode is active.
P..... Number of the program currently selected.
Message "In position" - "Execution" - "Interrupted" - "RESET".
PLC messages.
3. This window shows the CNC messages.
4. This window may show the following data:
X, Z coordinates of the axes. The Ø symbol indicates that the axis is working in diameter.
In small characters, the axis coordinates referred to machine reference zero. These values are
useful when letting the user define a tool change point (see zone 6) The CNC shows this data
when text 33 of program 999997 has not been defined.
The coordinates of the auxiliary axes that are defined.
The "C" axis will only be displayed when it is enabled (G15) and may be governed manually with
the jog keys [C+] and [C-]. Being the X-C plane active, the coordinates shown correspond to the
transformed coordinates; not to the machine coordinates.
The actual spindle rpm (S symbol) or the actual rpm of the second spindle (S2 symbol).
5. The information shown in this window depends on the position of the left switch.
In all cases, it shows the axis feedrate "F" currently selected and the % of F being applied.
When feed-hold is active, the color of the feedrate value changes.
1
2 3
4
5
6
7
9
15:28:42 SBK P000002 IN POSITION
X
Z
S
00044.000
-00443.331
0
REFERENCE ZERO X 0000.000
REFERENCE ZERO Z 0000.000
00025.000
00000.013
00014.480
F 0100.000
% 080
T 02
S 0100
D 12
CHANGE POSITION
X 25.000 Z 85.000
% 115
SMAX 1000 RANGE 1
020.0000
8
10
Page 35
Operating manual
CNC 8055
CNC 8055i
OPERATING IN JOG MODE
2.
·TC· OPTION
SOFT: V02.2X
·35·
Introduction
Here are all the possible cases.
6. This window shows, in large characters, the selected tool number "T" and, in small characters,
the "D" offset associated with the tool. If the tool number and the offset number are the same,
the CNC will not show the "D" value. The window also shows a drawing of the location code
(shape) associated with the tool.
This window also shows the coordinates of the tool change point referred to machine reference
zero. The CNC does not show this window when text 47 of p rogram 9999 97 has not been defined.
7. This window shows everything related to the spindle:
The theoretical turning speed that is selected; "S" value when constant turning speed and "CSS"
value when working at constant surface speed.
The spindle status. It is represented with an icon and may be turning cl ockwise, counterclockwise
or stopped.
The % of spindle speed being applied.
The maximum spindle rpm.
The active spindle speed gear (range). The CNC does not show this data when text 28 of program
999997 has not been defined.
8. Spindle angular increment when working in spindle orientation mode.
9. When accessing a work cycle, this window shows the help text associated with the selected icon.
That help text must be defined in program P999997 and edited in the desired language. See
chapter "1 General concepts".
10.Reserved.
Displaying the active PLC messages
At the screen, press [+] of the alphanumeric keyboard, the CNC shows a window with all the active
PLC messages. Besides, this window is also displayed whenever there is a program in execution.
The [] [] [PAGE UP] [PAGE DOWN] keys are used to move around the messages. The [ESC]
key is used to close the window.
The window is only displayed when there are more than one active message.
Direct access to the oscilloscope
The oscilloscope may be accessed from the standard screen by pressing "7" and then "1" as long
as no data is being written into any field.
100
10
1
100
10
1
1000
10000
JOG
100
10
1
100
10
1
1000
10000
JOG
100
10
1
100
10
1
1000
10000
JOG
100
10
1
100
10
1
1000
10000
JOG
100
10
1
100
10
1
1000
10000
JOG
100
10
1
100
10
1
1000
10000
JOG
15:28:42 IN POSITION
X
Z
S
00044.000
-00443.331
115
TO GO X 0000.000
TO GO Z 0000.000
F 0100.000
% 080
S 0100
% 115
SMAX 1000
RANGE 1
T 02
D 12
CHANGE POSITION
X 25.000 Z 85.000
F 0100.000
% 080
x10
F 0100.000
% 080
100
F 0100.000
% 080
Page 36
·36·
Operating manual
CNC 8055
CNC 8055i
2.
OPERATING IN JOG MODE
·TC· OPTION
SOFT: V02.2X
Introduction
2.1.2 Description of the special screen of the TC mode
The special screen of the TC mode offers the following data:
1. Clock.
2. This window may show the following data:
SBK When "single block" execution mode is selected.
DNC When the DNC mode is active.
P..... Number of the program currently selected.
Message "In position" - "Execution" - "Interrupted" - "RESET".
PLC messages.
3. This window shows the CNC messages.
4. This window shows the lines of the program currently selected.
5. The X, Z, C axes have the following fields:
The spindle (S) has the following fields:
The auxiliary axes only show the real current position of the axis.
Being the X-C plane active, the coordinates shown in the "Actual" field correspond to the
transformed coordinates; not to the machine coordinates.
COMMAD It indicates the programmed coordinate or position that the
axis must reach.
ACTUAL It indicates the actual (current) position of the axis.
TO GO It indicates the distance which is left to run to the
programmed coordinate.
FOLLOWING ERROR Difference between the theoretical value and the real value
of the position.
THEORETICAL Programmed theoretical S speed.
RPM Speed in rpm.
M/MIN Speed in meters per minute.
FOLLOWING ERROR When working with spindle orientation (M19), it indicates
the difference between the theoretical and the real speeds.
15:28:42 SBK P000002 IN POSITION
M0
(MSG " " )
(IF P1 02 EQ 1 GOTO N10)
(IF P1 01 EQ 0 RET)
M3
(RET)
N10 M4
(RET)
G01 G18
M41
PARTC : 000000
CYTIME : 00:00:00:00
TIMER: : 000000:00:00
COMMAND
X 00020.000
Z 00089.520
C 00014.480
U 00025.000
THEORETICAL
ACTUAL
X 00020.000
Z 00089.520
C 00014.480
RPM M/MIN
TO GO
X 00000.000
Z 00000.000
C 00000.000
X 00000.000
Z 00000.000
C 00000.000
FOLLOWING ERROR
S 0.000 0 S 0.0000 S 0. 00 00 S 0.0000
B 00000.013
1
2 3
4
5
6
87
Page 37
Operating manual
CNC 8055
CNC 8055i
OPERATING IN JOG MODE
2.
·TC· OPTION
SOFT: V02.2X
·37·
Introduction
6. This window shows the status of the "G" functions and the auxiliary "M" functions that are active.
Likewise, it shows the value of the variables.
7. Reserved.
8. Reserved.
Displaying the active PLC messages
At the screen, press [+] of the alphanumeric keyboard, the CNC shows a window with all the active
PLC messages. Besides, this window is also displayed whenever there is a program in execution.
The [] [] [PAGE UP] [PAGE DOWN] keys are used to move around the messages. The [ESC]
key is used to close the window.
The window is only displayed when there are more than one active message.
Direct access to the oscilloscope
The oscilloscope may be accessed from the auxiliary screen by pressing "7" and then "1" as long
as no data is being written into any field.
PARTC It indicates the number of consecutive parts executed with the same part-
program.
Every time a new program is selected, this variable is reset to "0".
CYTIME It indicates the time elapsed while executing the part. It is given in "hours:
minutes: seconds: hundredths of a second" format.
Every time a part-program execution starts, even when repetitive, this variable
is reset to "0".
TIMER It indicates the count of the timer enabled by PLC. It is given in "hours: minutes:
seconds" format.
Page 38
·38·
Operating manual
CNC 8055
CNC 8055i
2.
OPERATING IN JOG MODE
·TC· OPTION
SOFT: V02.2X
Introduction
2.1.3 Selecting a program for simulation or execution
When selecting a part-program or operation saved as part of a part-program for simulation or
execution, the CNC selects that part-program and shows it highlighted next to the green "start"
symbol in the top center window.
When the top center window shows the part-program selected next to the green "start" symbol, the
CNC acts as follows:
• If [START] is pressed, the CNC executes the part-program that is selected.
• If [CLEAR] is pressed, the CNC de-selects the part-program and removes it from the top center
window.
15:28:42
X
Z
S
00044.000
-00443.331
115
REFERENCE ZERO X 0000.000
F 0100.000
% 080
T 02
S 0100
D 12
CHANGE POSITION
X 25.000 Z 85.000
% 115
SMAX 1000
RANGE 1
P000002
REFERENCE ZERO Z 0000.000
15:28:42
M0
(MSG " " )
(IF P102 EQ 1 GOTO N10)
(IF P101 EQ 0 RET)
M3
(RET)
N10 M4
(RET)
G01 G18
M41
PARTC : 000 000
CYTIME : 00:00:00:00
TIMER: : 000000:00:00
COMMAND
X 00020.000
Z 00000.000
THEORETICAL
ACTUAL
X 00020.000
Z 00000.000
RPM M /MIN
TO GO
X 00000.000
Z 00000.000
X 00000.000
Z 00000.000
FOLLOWING ERROR
S 0. 0000 S 0.0000 S 0. 0000 S 0.0000
P000002
Page 39
Operating manual
CNC 8055
CNC 8055i
OPERATING IN JOG MODE
2.
·TC· OPTION
SOFT: V02.2X
·39·
Axis control
2.2 Axis control
2.2.1 Work units
When accessing the TC mode, the CNC assumes the work units «mm or inches", «mm/min. or
mm/rev», «radius or diameter» etc. selected by machine parameter.
To modify those values, access the T mode and change the corresponding machine parameter.
2.2.2 Coordinate preset
The coordinates must be preset on one axis at a time proceeding as follows:
1. Press the key of the desired axis, [X] or [Z].
The CNC will highlight the coordinate of that axis indicating that it is selected.
2. Key in the value to preset the axis.
To quit the preset mode, press [ESC].
3. Press [ENTER] for the CNC to assume that value as the new value for the point.
The CNC requests confirmation of the command. Press the [ENTER] to confirm it or [ESC] to
quit the preset mode.
2.2.3 Managing the axis feedrate (F)
To set a particular axis feedrate value, proceed as follows:
1. Press the [F] key.
The CNC will highlight the current value that it is selected.
2. Key in the desired new feedrate value.
To quit the preset selection mode, press [ESC].
3. Press [START] for the CNC to assume that value as the new value for axis feedrate.
Page 40
·40·
Operating manual
CNC 8055
CNC 8055i
2.
OPERATING IN JOG MODE
·TC· OPTION
SOFT: V02.2X
Machine reference (home) search
2.3 Machine reference (home) search
Home search may be done in 2 ways:
• Homing all the axes.
• Homing a single axis.
Homing all the axes
To home all the axes, press [ZERO].
The CNC requests confirmation of the command (text 48 of program 999997). Press [START], the
CNC will execute the home search subroutine defined by the OEM in general machine parameters
P34 (REFPSUB).
Homing a single axis
To home a single axis, press the key of the desired axis and the key for home search.
In either case, the CNC requests confirmation of the command (text 48 of program 999997).
ZERO
ZERO
After searching home this way, the CNC will maintain the part zero or zero offset active at the time.
A home search subroutine (general machine parameter P34 other than 0) must be defined when using
this method. Otherwise, the CNC will display the corresponding error.
i
It homes the X axis.
It homes the Z axis.
X
AR
ZERO
Z
J"
ZERO
After searching home this way, the CNC will not maintain the part zero or zero offset active at the time
and assumes the machine reference zero as the new part zero.
i
Page 41
Operating manual
CNC 8055
CNC 8055i
OPERATING IN JOG MODE
2.
·TC· OPTION
SOFT: V02.2X
·41·
Zero offset table
2.4 Zero offset table
It is possible to manage the zero offset table from the conversational mode (G54.... G59, G159N7
... G159N20). This table contains the same values as that of the conversational mode.
Press the [ZERO] key to access the zero offset table as well as to get out of it. The zero offset table
may be accessed in the following ways.
• From the standard screen, as long as no axis is selected. The CNC will request confirmation
of the command.
• From ISO mode, when the "zero offsets and presets" cycle is selected.
The zero offset table looks like this. It shows all the offsets, PLC offset included, and their value in
each axis.
When scrolling the focus through the table, the elements appear in different colors as follows.
How to edit the table data
The following operations are possible in the zero offset table. Press [ENTER] to validate any
changes.
• Editing a zero offset.
It is edited one axis at a time. Select a data with the focus and edit its value. If the magnifying
glass is placed on top of an offset (G54 ... G59, G159N7 ... G159N20), editing start on the first
axis of that offset.
• Load the active zero offset into the table.
Position the magnifying glass over the offset you wish to define (G54 ... G59, G159N7 ...
G159N20) and click on the [RECALL] key. The active preset is saved in the selected zero offset.
If instead of placing the focus on a zero offset, it is placed on one of the axes, only that axis will
be affected.
• Deleting a zero offset.
Position the magnifying glass over the offset that you wish to erase (G54 ... G59, G159N7 ...
G159N20) and click on the [CLEAR] key. All the axes of that zero offset are reset to zero.
If instead of placing the focus on a zero offset, it is placed on one of the axes, only that axis will
be affected.
Color Meaning
Green background.
Text in white.
The real value of the table and the value shown on the screen are the same.
Red background.
White text.
The real value of the table and the value shown on the screen are NOT the same.
The value on the table has been changed, but it has not been validated. Press
[ENTER] to validate the change.
Blue background. The zero offset is active.
Two origins may be active simultaneously, one absolute (G54 ... G57, G159N7
... G159N20) and another incremental (G58-G59).
PLC
G54
G55
G56
G57
G59
G58
XZ
V
0.0000
0.0000
0.0000
0.0000
0.0000
0.0000
0.0000
0.0000
0.0000
0.0000
0.0000
0.0000
0.0000
0.0000
0.0000
0.0000
0.0000
0.0000
0.0000
0.0000
0.0000
Page 42
·42·
Operating manual
CNC 8055
CNC 8055i
2.
OPERATING IN JOG MODE
·TC· OPTION
SOFT: V02.2X
Jog movement
2.5 Jog movement
When making a move in manual, both in jog and with handwheels, the moving axis appears in
reverse video.
• With gantry axes, only the master axis is highlighted.
• With a path handwheel, no axis is highlighted; but it is in path-jog.
2.5.1 Moving an axis to a particular position (coordinate)
The movements of axes to a particular coordinate are made one at a time as follows
[X] Target coordinate [START]
[Z] Target coordinate [START]
2.5.2 Incremental movement
Turn the JOG switch to one of the JOG positions.
The incremental movement must be made one axis at a time. To do that, press the JOG keys for
the direction of the axis to be jogged.
Every time a key is pressed, the corresponding axis moves the amount set by the switch. This
movement is made at the selected feedrate (F).
Switch position Distance
1 0.001 mm or 0.0001 inches
10 0.010 mm or 0.0010 inches
100 0.100 mm or 0.0100 inches
1000 1.000 mm or 0.1000 inches
10000 10.000 mm or 1.0000 inches
100
10
1
100
10
1
1000
10000
JOG
100
10
1
100
10
1
1000
10000
JOG
Page 43
Operating manual
CNC 8055
CNC 8055i
OPERATING IN JOG MODE
2.
·TC· OPTION
SOFT: V02.2X
·43·
Jog movement
2.5.3 Continuous jog
Place the movement selector in the continuous-jog position and select at the feedrate override switch
(FEED) the percentage (0% to 120%) of the feedrate to be applied.
The continuous jog must be made one axis at a time. To do that, press the JOG keys for the direction
of the axis to be jogged.
The axis moves at a feedrate equal to the selected percentage (0% to 120%) of feedrate "F".
Depending on the status of the general logic input "LATCHMAN", the movement will be carried out
as follows:
• If the PLC sets this mark low, the axis will be jogged while pressing the corresponding Jog key.
• If the PLC sets this mark high, the axes will start moving from the moment the JOG key is pressed
until the same is pressed again, or another JOG key is pressed. In this case, the movement will
be transferred to that indicated by the new key.
The following cases are possible when working with "F" in mm/rev:
• The spindle is running.
• The spindle is stopped, but a spindle speed S has been selected.
• The spindle is stopped and no spindle speed S has been selected.
The spindle is running:
The spindle is stopped, but a spindle speed S has been selected:
The spindle is stopped and no spindle speed S has been selected:
If while jogging an axis, the rapid key is pressed, the axis will move at the maximum
feedrate possible, set by axis machine parameter "G00FEED". This feedrate will be
applied while that key is kept pressed and the previous feedrate will be restored when
that key is released.
The CNC moves the axes at the programmed F.
The CNC calculates the feedrate F in mm/min for the theoretical S and moves the
axis.
For example if "F 2.000" and "S 500":
F (mm/min) = F (mm/rev) x S (rpm) = 2 x 500 = 1000 mm/min.
The axis moves at a feedrate of 1000 mm/min.
If F = 0, the CNC moves the axes in rapid.
If F is other than 0, the axes can only be moved by pressing the rapid key and
an axis key. The CNC moves the axis in rapid.
If the axis to be jogged does not belong to the active plane, the movement is
carried out in mm/minute; thus, it is not necessary to program an S at the spindle.
Also, if any axis of the plane is the Y axis, it is not necessary either to program
the S for jog movements in any axis, regardless of whether it belongs to the plane
or not.
This is especially interesting for auxiliary axes, center rests and tailstocks,
because, in those cases, the S has no effect.
100
10
1
100
10
1
1000
10000
JOG
100
10
1
100
10
1
1000
10000
JOG
0
2
4
10
20
30
405060
70
80
90
100
110
120
FEED
%
0
2
4
10
20
30
405060
70
80
90
100
110
120
FEED %
S 0500
% 115
S 0500
% 115
Page 44
·44·
Operating manual
CNC 8055
CNC 8055i
2.
OPERATING IN JOG MODE
·TC· OPTION
SOFT: V02.2X
Jog movement
2.5.4 Path-jog
The "path jog" mode acts when the switch is in one of the continuous or incremental jog positions.
This feature may be used to act upon the jog keys of an axis to move both axes of the plane at the
same time for chamfering (straight sections) and rounding (curved sections). The CNC assumes
as "Path jog" the keys associated with the X axis.
While in jog mode and having selected path-jog, the CNC shows the following information:
For a linear movement (top figure), the path angle must be defined and for an arc (bottom figure),
the center coordinates must be indicated. To define these variables, press the [F] key and then one
of these keys: [] [] [] [].
This feature must be managed from the PLC. This feature is usually activated and deactivated by
means of an external push-button or a key configured for that purpose, as well as the selection of the
type of path.
i
The next example uses the [O2] key to activate and deactivate the path-jog mode and the
[O3] key to indicate the type of movement.
Activate / deactivate the path-jog mode.
DFU B29 R561 = CPL M5054
It selects the type of movement, straight section or arc section.
DFU B31 R561 = CPL M5053
100
10
1
100
10
1
1000
10000
JOG
100
10
1
100
10
1
1000
10000
JOG
15:28:42
IN POSITION
X
Z
S
00044.000
-00443.331
115
TO GO X 0000.000
TO GO Z 0000.000
F 0100.000
% 080
T 02
S 0100
% 115
SMAX 1000
RANGE 1
F 0100.000
% 080
x10
30.000
F 0100.000
% 080
x10
Xc 15.512
Zc 22.345
Xc
Zc
Page 45
Operating manual
CNC 8055
CNC 8055i
OPERATING IN JOG MODE
2.
·TC· OPTION
SOFT: V02.2X
·45·
Jog movement
Operation in path-jog mode
The "path jog" mode is only available with the X axis keys. When pressing one of the keys associated
with the X axis, the CNC behaves as follows:
The rest of the jog keys always work in the same way, whether "path jog" is on or off. The rest of
the keys move only the axis and in the indicated direction.
The movements in path-jog may be aborted by pressing the [STOP] key or setting the jog switch
to one of the handwheel positions.
Considerations about the jog movements
This mode assumes as axis feedrate the one selected in jog mode and it will also be affected by
the feedrate override switch. If F0 is selected, it assumes the one indicated by machine parameter
"JOGFEED (P43)". This mode ignores the rapid jog key.
Path-jog movements respect the travel limits and the work zones.
Switch position Path-jog Type of movement
Continuous jog Deactivated Only the axis and in the indicated direction
Activated Both axes in the indicated direction and along the indicated path
Incremental jog Deactivated Only the axis, the selected distance and in the indicated direction
Activated Both axes, the selected distance and in the indicated direction,
but along the indicated path
Handwheel It ignores the keys.
Page 46
·46·
Operating manual
CNC 8055
CNC 8055i
2.
OPERATING IN JOG MODE
·TC· OPTION
SOFT: V02.2X
Jog movement
2.5.5 Movement with an electronic handwheel
This option may be used to govern the movements of the machine using an electronic handwheel.
To do that, turn the left switch to any of the handwheel positions.
The positions available are 1, 10 and 100; they indicate the multiplying factor being applied besides
the internal x4 to the feedback pulses supplied by the electronic handwheel.
The machine has an electronic handwheel
Once the desired switch position has been selected, press one of the JOG keys for the axis to be
jogged. The bottom of the screen shows the selected axis in small characters and next to the
handwheel symbol.
When using a FAGOR handwheel with an axis selector button, the axis may be selected as follows:
• Push the button on the back of the handwheel. The CNC select the first axis and it highlights it.
• When pressing the button again, the CNC selects the next axis and so on in a rotary fashion.
• To deselect the axis, hold the button pressed for more than 2 seconds.
Once the axis has been selected, it will move as the handwheel is being turned and in the direction
indicated by it.
The machine has two or three electronic handwheels
Each axis will move as the corresponding handwheel is being turned according to th e switch positi on
and in the direction indicated by it.
When the machine has a general handwheel and individual handwheels (associated with each axis
of the machine), the individual handwheels have the highest priority; i.e. when moving an individual
handwheel, the CNC will ignore the general handwheel.
Switch position Distance per turn
1 0.100 mm or 0.0100 inches
10 1.000 mm or 0.1000 inches
100 10.000 mm or 1.0000 inches
100
10
1
100
10
1
1000
10000
JOG
100
10
1
100
10
1
1000
10000
JOG
It may happen that depending on the turning speed and the selector switch position, the CNC be
demanded a faster feedrate than the maximum allowed (axis machine parameter "G00FEED"). The
CNC will move the axis the indicated distance but at the maximum feedrate allowed.
i
Page 47
Operating manual
CNC 8055
CNC 8055i
OPERATING IN JOG MODE
2.
·TC· OPTION
SOFT: V02.2X
·47·
Jog movement
2.5.6 Feed handwheel
Usually, when making a part for the first time, the machine feedrate is controlled by means of the
feedrate override switch.
From this version on, it is also possible to use the machine handwheels to control that feedrate. This
way, the machining feedrate will depend on how fast the handwheel is turned.
The following CNC variables return the number of pulses the handwheel has turned.
HANPF provides the number of pulses of the 1st handwheel.
HANPS provides the number of pulses of the 2nd handwheel.
HANPT provides the number of pulses of the 3rd handwheel.
HANPFO provides the number of pulses of the 4th handwheel.
This feature must be managed from the PLC. Usually, this feature is turned on and off using an external
push button or key configured for that purpose.
i
Page 48
·48·
Operating manual
CNC 8055
CNC 8055i
2.
OPERATING IN JOG MODE
·TC· OPTION
SOFT: V02.2X
Jog movement
2.5.7 Path-handwheel
The "path handwheel" mode acts when the switch is in one of the handwheel positions. With this
feature, it is possible to jog two axes of the plane at the same time along a linear path (chamfer)
or circular path (rounding) with a single handwheel. The CNC assumes as the path handwheel the
general handwheel or, when this one is missing, the one associated with the X axis.
While in handwheel mode and having selected path-handwheel, the CNC shows the following
information:
For a linear movement (top figure), the path angle must be defined and for an arc (bottom figure),
the center coordinates must be indicated. To define these variables, press the [F] key and then one
of these keys: [] [] [] [].
Operation in path-handwheel mode
When selecting the path handwheel mode, the CNC behaves as follows.
• If there is a general handwheel, it will be the one working in path handw heel mode. The individual
handwheels, if any, will remain associated with the corresponding axes.
• If there is no general handwheel, the individual handwheel associated with the X axis then works
in path-handwheel mode.
The movements in path-handwheel may be aborted by pressing the [STOP] key or setting the jog
switch to one of the continuous or incremental positions.
This feature must be managed from the PLC. This feature is usually activated and deactivated by
means of an external push-button or a key configured for that purpose, as well as the selection of the
type of path.
i
The next example uses the [O2] key to activate and deactivate the path-handwheel mode and
the [O3] key to indicate the type of movement.
Activate / deactivate the path-handwheel mode.
DFU B29 R561 = CPL M5054
It selects the type of movement, straight section or arc section.
DFU B31 R561 = CPL M5053
100
10
1
100
10
1
1000
10000
JOG
100
10
1
100
10
1
1000
10000
JOG
15:28:42
IN POSITION
X
Z
S
00044.000
-00443.331
115
TO GO X 0000.000
TO GO Z 0000.000
F 0100.000
% 080
T 02
S 0100
% 115
SMAX 1000
RANGE 1
F 0100.000
% 080
x10
30.000
F 0100.000
% 080
x10
Xc 15.512
Zc 22.345
Xc
Zc
Page 49
Operating manual
CNC 8055
CNC 8055i
OPERATING IN JOG MODE
2.
·TC· OPTION
SOFT: V02.2X
·49·
Tool control
2.6 Tool control
The standard screen of the TC mode offers the following tool data.
This window displays the following information:
• In large characters, the tool "T" number currently selected and a graphic representation of its tip.
• The "D" offset number associated with the tool.
• The "S" rpm that are selected for the live tool. This value is only shown when a live tool has been
selected.
• The position values of the tool change point. The CNC does not show this window when text
47 of program 999997 has not been defined.
To select another tool, follow these steps:
1. Press the [T] key.
The CNC highlights the tool number.
2. Key in the number of the tool to be selected.
To quit the preset selection mode, press [ESC].
3. Press [START] for the CNC to select the new tool.
The CNC will manage the tool change. Once the new tool has been selected, the CNC refreshes
the graphic representation for the location code (shape) associated with the new tool.
Another offset may be assigned to the tool temporarily without modifying the one associated with it.
1. To access the "D" field, press [T] and [].
2. Key in the number of the desired tool offset and press [START].
The CNC temporarily assumes the new offset for the current tool. The internal table is not
modified, the tool’s associated offset is still the one assigned to it when it was calibrated.
T 02
D 12
CHANGE POSITION
X 25.000 Z 85.000
S 150
T 02
D 12
CHANGE POSITION
X 25.000 Z 85.000
S 150
Page 50
·50·
Operating manual
CNC 8055
CNC 8055i
2.
OPERATING IN JOG MODE
·TC· OPTION
SOFT: V02.2X
Tool control
2.6.1 Tool change
Depending on the type of tool changer, the following options are possible:
• Machine with automatic tool changer.
• Machine with manual tool changer.
In either case, the CNC acts as follows:
• The CNC executes the subroutine associated with the tool change (general machine parameter
P60 "TOOLSUB").
• The CNC sends to the PLC all the necessary information for it to manage the tool change.
• The CNC assumes the new tool values (offsets, geometry, etc).
Example of how to manage a manual tool changer.
• Subroutine 55 is defined as the subroutine associated with the tools.
General machine parameter P60 "TOOLSUB" = 55.
The subroutine associated with the tools may contain the following information:
• The tool is selected after executing the subroutine.
General machine parameter P71 "TAFTERS" = YES.
• The movement to the change point only takes place when executing an operation or cycle of
the TC mode.
• Once the subroutine is completed, the CNC executes function T??, sends to the PLC all the
necessary information for it to manage the tool change and assumes the new to ol value s (offsets,
geometry, etc.).
(SUB 55)
(P100 = NBTOOL)
; Assigns the requested tool number to P100.
(P101 = MS3)
; If spindle counterclockwise P102=1.
G0 G53... XP?? ZP??
; Movement to the tool change point.
M5
; Spindle stop.
(MSG "SELECT T?P100 AND PRESS START")
; Message to select the tool change.
M0
; Stop the program stop and wait for START to be pressed.
(MSG "" "")
; Deletes previous message.
(IF P102 EQ 1 GOTO N10)
; Restores the spindle turning direction.
(IF P101 EQ 0 RET)
M3
(RET)
N10 M4
(RET)
When a cycle has been selected (CYCEXE other than 0)
The program is being executed (OPMODA bit 0 = 1).
Page 51
Operating manual
CNC 8055
CNC 8055i
OPERATING IN JOG MODE
2.
·TC· OPTION
SOFT: V02.2X
·51·
Tool control
2.6.2 Variable tool change point
If the manufacturer so wishes, he can let the user define the tool change point every time. Obviously,
this feature depends on the type of machine and type of tool changer.
This feature may be used to change the tool next to the part, thus avoiding movements to a tool
change point located far away from it.
To do this:
• Define the text 47 of program 999997 so the CNC requests the X, Z coordinates of the tool
change point.
For example: ;47 $CHANGE POSITION
These coordinates must be referred to machine zero point, so the zero offsets do not affect the
tool change point. Therefore, the CNC can show, next to the X, Z coordinates and in small
characters, the coordinates of the axes referred to machine reference zero.
• Text 33 of program 999997 must be defined so the CNC shows the coordinates of the axes
referred to machine reference zero.
For example: ;33 $MACHINE ZERO
Since the operator can change the tool change point at any time, the subroutine associated with
the tools must consider those values. Arithmetic parameters P290 and P291 contain the values set
by the operator as tool change position in X and Z respectively.
In subroutine 55 of the previous section, the line setting the movement to the tool change point must
be modified:
Where it says:
G0 G53 XP??? ZP??? ; Movement to the tool change point.
It must say:
G0 G53 XP290 ZP291 ;User-defined movement to the change point.
Define the coordinates of the tool change point (X, Z)
1. Press the [T] key to select the «T» field.
2. Then press the [X], [Y] or [Z] key of the desired axis or the [] [] [] [] keys.
3. After placing the cursor on the coordinates of the axis to be defined, define the desired values.
After placing the cursor on the coordinates of the axes to be defined, the value is entered in one
of the following ways.
• Entering the value manually. Key in the desired value and press [ENTER].
• Assign the current machine position.
Jog the axis with the handwheel or the JOG keys up to the desired point. Press [RECALL] so
the selected data assumes the value shown in the top right window and press [ENTER].
The top right window shows the tool position at all times.
Arithmetic parameter P290.
Change position in X.
Arithmetic parameter P291.
Change position in Z.
T 02
D 12
CHANGE POSITION
X 25.000 Z 85.000
S 150
T 02
D 12
CHANGE POSITI ON
X 25.000 Z 85.000
S 150
Page 52
·52·
Operating manual
CNC 8055
CNC 8055i
2.
OPERATING IN JOG MODE
·TC· OPTION
SOFT: V02.2X
Tool calibration
2.7 Tool calibration
The calibration mode can have several editing levels. The second level will only be available when
using a table-top probe installed on the machine.
What can be done in tool calibration mode
The data that may be modified from the calibration cycles depend on when this mode is accessed.
The following limitations must be borne in mind when accessing the tool calibration mode with a
program in execution or from tool inspection.
Without a program in execution nor in tool inspection.
When editing the active tool, it is possible:
• Modify all the data.
• Change the active tool (T ?? + [START]).
When NOT editing the active tool, it is possible:
• Modify all the data except the part dimensions.
• Change the active tool (T ?? + [START]).
Program in execution or interrupted.
When editing the active tool, it is possible:
• To modify the I and K data.
• Select another tool (T?? + [RECALL]) and modify the I and K data.
When NOT editing the active tool, it is possible:
• To modify the I, K and D data.
• Select another tool (T?? + [RECALL]) and modify the I, K and D data.
Program in tool inspection.
When editing the active tool, it is possible:
• To modify the I and K data.
• Select another tool (T?? + [RECALL]) and modify the I and K data.
• Change the active tool (T ?? + [START]).
When NOT editing the active tool, it is possible:
• To modify the I, K and D data.
• Select another tool (T?? + [RECALL]) and modify the I, K and D data.
• Change the active tool (T ?? + [START]).
This mode may be used to define the tools and calibrate them. The tools may be
calibrated with or without using a probe.
This mode is also available while executing a program and during tool inspection.
Each level has its own screen and the main window of the cycle indicates, with tabs, the
available levels and which one is selected. To change levels, use the [LEVEL CYCLE]
key or the [page up] and [page down] keys to scroll up and down through the various
levels.
LEVEL
CYCLE
Page 53
Operating manual
CNC 8055
CNC 8055i
OPERATING IN JOG MODE
2.
·TC· OPTION
SOFT: V02.2X
·53·
Tool calibration
2.7.1 Define the tool in the tool table (level 1)
When accessing this level, the CNC shows the following screen.
1. Indicating the selected work mode: "Tool calibration".
2. Graphic assistance for tool calibration.
3. Help graphics for defining tool geometry.
4. Current machine status.
Real X Z coordinates, real axis feedrate F, real spindle speed S and currently selected tool T.
5. Tool number, tool offset number, location code (shape) and tool family.
6. Length values defined for this tool.
7. Values for the geometry of the tool.
Define the tool data
Proceed as follows to define a tool in the tool table:
Select the number of the tool to be defined.
1. Press the [T] key to select the "T" field.
2. Key in the desired tool number and press [RECALL].
If the tool is defined, the CNC will show the values stored in the table. If the tool is not defined,
the CNC assigns an offset with the same number to it and all the data is reset to 0.
Select the number of the offset tool to be associated with this tool.
1. The "D" field must be selected. If it is not, use the [] key.
2. Key in the desired offset number to be associated with the tool and press [ENTER].
Define the tool dimensions.
The data for the tool is the following.
Even if the tool dimensions are known, it is recommended to measure it. See "2.7.2 Manual tool
calibration with/without a probe (level 1)" on page 56.
Once it is measured, the CNC updates the X, Z fields and sets the I and K data to 0.
To define these values, select the corresponding field with the [ ] [ ] [] [] keys, key in the desired
value and press [ENTER].
15:28:42
Z123.5000
X 45.000
Z - ENTER
X 00044.000 Z -003 97.490
F 1.000 S 150 T 3
T0002 D002
Family Shape
F3
TOOL CALIBRATION
X 0.0000
I 0.0000
Z 0.0000
K 0.0000
X - ENTER
Z - ENTER
Cutter angle
Cutter width
Cutting angle
Tool nose radius
A 0.0000
B 0.0000
C 0.0000
R 0.0000
Tool calibration
Geometry
C
R
A
B
A=90
A=90
B=2R
1
2
3
4
5
6
7
X Tool's X dimension (in radius).
Z Tool's Z dimension.
I X wear offset (in diameter).
K Z wear offset.
15:28:42
Z123.5000
X 45.000
Z - ENTER
X 0.0000
I 0.0000
Z 0.0000
K 0.0000
X - ENTER
Z - ENTER
Tool calibration
Page 54
·54·
Operating manual
CNC 8055
CNC 8055i
2.
OPERATING IN JOG MODE
·TC· OPTION
SOFT: V02.2X
Tool calibration
Defining the tool type.
Define the location code of the tool.
Place the cursor over the icon for tool type and press the two-color key. The available
tool types are:
Place the cursor over the icon for tool type and press the two-color key. The available
tool types are:
*
*
C
R
A
B
F0
F1 F2 F3
F4
F5F6F7
F8
F9
X
X
Z
Z
F1F9F2 F3
F4
F5F6F7
F8
F0
X
Z
X
Z
F41
F41
F42
F42
F43
F43
F51
F51
F58 F58
F57
F57
F47
F47
F46
F46
F45
F45
F53
F53
F54 F54
F55
F55
F59 F59
F49
F49F40
F40
F50 F50
A=90
B=2R
C=0
R
X
Z
X
Z
F68
F62
F64
F66
F68
F62
F66
F64
C
A
B
R
X
Z
X
Z
F21
F21
F22
F22
F23
F23F27
F27
F26
F26
F25
F25
F31
F31
F38 F38
F37
F37F33
F33
F34 F34
F35
F35
C=90
A=90
R=0
B
X
Z
X
Z
F20
F20
F10 F10
F30
F30
A=180
C=0
R
B
R
B
A
C
Page 55
Operating manual
CNC 8055
CNC 8055i
OPERATING IN JOG MODE
2.
·TC· OPTION
SOFT: V02.2X
·55·
Tool calibration
Define the rest of the data related to the tool.
The right window shows the tool geometry values and the left window shows help graphics. To define
one of these values, select the corresponding field, key in the desired value and press [ENTER].
15:28:42
Cutter angle
Cutter width
Cutting angle
Tool nose radius
A 0.0000
B 0.0000
C 0.0000
R 0.0000
Geometry
C
R
A
B
A=90
A=90
B=2R
A Cutter angle.
B Cutter width.
C Cutting angle.
R Tool radius.
Page 56
·56·
Operating manual
CNC 8055
CNC 8055i
2.
OPERATING IN JOG MODE
·TC· OPTION
SOFT: V02.2X
Tool calibration
2.7.2 Manual tool calibration with/without a probe (level 1)
Before measuring the tool, it must be defined in the tool table. See "2.7.1 Define the tool in the tool
table (level 1)" on page 53.
There are 2 ways to calibrate a tool.
• When having a tool setting table.
Use the window that shows the tool dimensions to define that data. Define the X Z dimensions
and the I, K wear.
• When not having any measuring device.
The measurements will be taken with the CNC. Use the window for tool calibration.
Manual tool calibration with/without a probe
When using a probe for calibrating, one must define the approach distance "", the approach
feedrate "F" and the probe side to be probed. If "
" not defined, it will take this data from general
machine parameter "PRBMOVE". Likewise, If "F" not defined, it will take this data from axis machine
parameter "PRBFEED".
Once probing is completed, the screen updates the data.
Define the tool length or modify the length offsets
This window shows the dimensions assigned to the selected tool.
The X and Z data indicate the tool dimensions. I and K indicate the offset the CNC must apply to
compensate for tool wear.
The CNC adds the value of the "I" offset to X length and the value of the "K" offset to the Z length
to calculate the real dimensions (R+I, L+K) that must be used.
• Every time the X length or the Z length value is defined, the CNC sets the "I" and "K" fields to
0 respectively.
• The "I" and "K" data are accumulative. In other words, if the "I" has a value of 0.20 and the value
of 0.05 is entered, the CNC assigns the value of 0.25 (0,20+0,05) to the "I" field.
• If one sets I=0 or K=0, they are both reset to 0.
To change one of these values, select the corresponding field, key in the desired value and press
[ENTER].
In the manual tool calibration cycle, it is possible to calibrate the tool using a master part
or a probe. The type of calibration is defined with the following icon: Use the two-color
key to select one of them.
Tool calibration using a master part of known dimensions.
Tool calibration using a probe.
*
15:28:42
Z123.5000
X 45.000
Z - ENTER
X 0.0000
I 0.0000
Z 0.0000
K 0.0000
X - ENTER
Z - ENTER
Tool calibration
X Tool's X dimension (in radius).
Z Tool's Z dimension.
I X wear offset (in diameter).
K Z wear offset.
Page 57
Operating manual
CNC 8055
CNC 8055i
OPERATING IN JOG MODE
2.
·TC· OPTION
SOFT: V02.2X
·57·
Tool calibration
Tool calibration
Place a part of known dimensions in the spindle and define its dimensions in the left window.
To measure the tool, the tool must be selected on the machine. If it is not, press the [T] key, key in
the desired number of the tool to be calibrated and press [START].
Measuring the tool.
1. Approach the tool to the part, touch it with it along the X axis and press [X] + [ENTER].
2. Approach the tool to the part, touch it with it along the Z axis and press [Z] + [ENTER].
The tool has been calibrated. The CNC updates the X, Z data and sets the I and K to 0. The actual
tool length is (X+I) and (Z+K); the "I" must be given in diameter.
Modifying the tool data while executing a program
It is possible to modifying the tool values (dimensions and geometry) without interrupting the
execution of a program.
To exit this screen, press [ESC].
To do that, press the tool calibration key. The CNC will show the tool calibration screen
with all the data for the active tool and it will allow modifying its data or of any other tool.
Page 58
·58·
Operating manual
CNC 8055
CNC 8055i
2.
OPERATING IN JOG MODE
·TC· OPTION
SOFT: V02.2X
Tool calibration
2.7.3 Tool calibration with a probe (level 2)
This calibration level requires the purchase of the right software options purchased and the use of
a table-top probe.
Once the cycle has concluded, it updates the tool offset table with the length value X Z of the tool
offset that is currently selected. The I and K values are updated to 0.
Defining the cycle data
The following data must be defined.
• Tool number (T) and tool offset (D) to be calibrated.
• Safety distance (Ds) for probe approach.
• Probing feedrate (F).
Probe position.
In this zone, one must indicate whether the cycle assumes the probe position defined in the machine
parameters or the position defined in this zone. To select one of them, use the cursor to select the
"Machine parameters / Programmable parameters" field and press the two-color key.
TOOL WEAR MEASUREMENT
In this cycle, besides calibrating a tool, it is also possible to measure tool wear.
Using the tool wear measuring operation, the user can define the maximum tool wear value. After
several tool wear measuring probing operations, the wear will increase and when it exceeds the set
maximum value, the tool will be rejected.
To perform this cycle it is necessary to have a table-top probe, installed in a fixed position on the
machine and with its faces parallel to axes X, Y, Z.
When accessing this calibration level, the CNC shows the following information:
A. Indicating the selected work mode.
B. Graphic assistance for tool calibration.
C. Current machine status.
D. Tool number and associated offset.
E. Calibration data.
F. Type of operation and wear values.
G. Probe position.
This level may be saved as part of a part-program using the [P.PROG] key or executed using the
[START] key.
Page 59
Operating manual
CNC 8055
CNC 8055i
OPERATING IN JOG MODE
2.
·TC· OPTION
SOFT: V02.2X
·59·
Tool calibration
Defining the cycle data
The following data must be defined. Not all the data will always be available; the cycle will show the
necessary data according to the chosen operation.
• Safety distance (Ds) for probe approach.
• Probing feedrate (F).
• Icon to set the Y axis direction.
• Type of operation:
The cycle allows doing a measurement or a calibration. To select the desired operation, place
the cursor in the "Measurement / Calibration" field and press the two-color key. To take a
measurement, define the following data.
Imax Maximum tool length wear measurement along the X axis.
Kmax Maximum tool length wear measurement along the Z axis.
Jmax Maximum tool length wear measurement along the Y axis.
Stop / Chg Cycle behavior when exceeding the maximum wear permitted. Use the two-color
key to select one of them.
The "Stop" option interrupts the execution for the user to select another tool. With
the "Chg" option, the cycle replaces the tool with another one of the same family.
Measuring is only available when purchasing the software option: "Tool life monitoring".
• Probe position.
In this zone, one must indicate whether the cycle assumes the probe position defined in the
machine parameters or the position defined in this zone. To select one of them, use the cursor
to select the "Machine parameters / Programmable parameters" field and press the two-color
key.
Machine parameters: The cycle assumes the probe position defined in the machine
parameters.
Programmed parameters: The cycle assumes the probe position defined in the cycle (Xmax,
Xmin, Ymax, Ymin, Zmax, Zmin).
Actions after completing the tool wear measuring cycle
To activate the rejected tool, either because it has been replaced with another one or because it
will be used to keep working, the following options will be offered:
1. Go into the tool table in ISO mode and delete the actual (real) life of that tool.
2. Go into the tool table in ISO mode and write the desired value for the actual (real) life of that tool.
In this case, activating the tool requires the real life to be smaller than the nominal (rated) life
value. Otherwise, the tool will appear as expired (worn out) (status = E).
Page 60
·60·
Operating manual
CNC 8055
CNC 8055i
2.
OPERATING IN JOG MODE
·TC· OPTION
SOFT: V02.2X
Tool calibration
2.7.4 Probe calibration (level 3)
This calibration level requires the purchase of the right software options purchased and the use of
a table-top probe.
This cycle may be used to calibrate the sides of the table-top probe, installed in a fixed position of
the machine whose sides parallel to the X and Z axes. The probe position must be defined in the
corresponding machine parameters (PRB*MIN, PRB*MAX).
To execute the cycle, a master tool of known dimensions will be used whose values have been
previously entered in the selected offset.
The data obtained in the calibration are updated directly in machine parameters PRB*MIN and
PRB*MAX. To do this, program P99998 must be set as OEM.
Defining the cycle data
The following data must be defined.
• Tool number (T) and tool offset (D) used to define the dimensions of the master part.
• Safety distance (Ds) for probe approach.
• Probing feedrate (F).
Probe position.
In this zone, one must indicate whether the cycle assumes the probe position defined in the machine
parameters or the position defined in this zone. To select one of them, use the cursor to select the
"Machine parameters / Programmable parameters" field and press the two-color key.
Page 61
Operating manual
CNC 8055
CNC 8055i
OPERATING IN JOG MODE
2.
·TC· OPTION
SOFT: V02.2X
·61·
Tool calibration
2.7.5 Manual tool calibration without stopping the spindle
This feature may be used to manually calibrate the tool on a conversational lathe. It may be used
to calibrate tools without having to go back with the tool after performing a turning or facing operation.
Tool calibration is done without having to stop the spindle at each pass. It saves the tool position
in each touch and it applies the calibration by measuring the par t only once at the end of the process.
Operation
Follow these steps to manually calibrate the tool:
1. After placing the part in the spindle and start the spindle, perform a facing operation.
2. Place the focus on "MEMO Z" and press the two-color key to save the current position
(coordinate).
Besides pressing the two-color key, pressing the [INS] or [-] key also memorizes the current
position. Once the position has been saved, enable "APPLY Z".
3. Withdraw the tool along the Z axis.
4. Perform a turning operation, place the focus on "MEMO X" and press the two-color key to save
the current position (coordinate).
Besides pressing the two-color key, pressing the [INS] or [-] key also memorizes the current
position.
5. Withdraw the tool along the X axis.
6. Stop the spindle and measure the resulting diameter of the turning operation just done.
The memorized positions are kept until a new calibration is applied or until quitting the tool cycle.
When quitting the cycle, a message warns that the saved data may get lost.
7. After filling the data out, the calibration may be applied on each axis (APPLY X or APPLY Z) or
on all the axes whose position has been memorized (APPLY ALL) so it assumes the new
calculated offsets. This is also possible with the Y axis.
It is also possible to delete the memorized position by pressing the [CLEAR] key when the focus
is on APPLY X, APPLY Y, APPLY Z or APPLY ALL. This way, a position may be corrected without
having to exit the screen.
The following hotkeys may be used to access the data quickly:
• The X, Y, Z keys give access to the fields for the part measurements before machining and to
the tool offsets for each axis.
• The M key gives access to the "MEMO" option used to memorize the positions.
• The A key gives access to the "APPLY" option used to apply the calibration.
Set bit 13 of general machine parameter CODISET (P147) = 0 to enable this calibration.
Page 62
·62·
Operating manual
CNC 8055
CNC 8055i
2.
OPERATING IN JOG MODE
·TC· OPTION
SOFT: V02.2X
Live tool
2.8 Live tool
When a live tool has been selected, the standard screen of the TC mode offers the following
information:
Proceed as follows to select the "S" rpm of the live tool:
1. Press the [T] key to select the "T" field.
2. Press the [S] key or the [] key to select the "S" rpm of the live tool.
3. Entering the value manually. Key in the desired value and press [ENTER].
The keys for the live tool are:
Considerations about the live tool
The following considerations must be borne in mind when the machine has a live tool:
• Set one of general parameters P0 to P9 with a value of 13.
• The location code (shape) of the live tool must be 10, 20 or 30.
• The PLC must manage the keys for the live tool.
Every time one of these keys is pressed, the CNC updates the corresponding register bit.
bit 7 of register 561 (B7 R561)
bit 3 of register 562 (B3 R562)
bit 5 of register 562 (B5 R562)
T 02
D 12
CHANGE POSITION
X 25.000 Z 85.000
S 150
T 02
D 12
CHANGE POSITI ON
X 25.000 Z 85.000
S 150
Turns clockwise.
Turns counterclockwise.
Stops turning.
Page 63
Operating manual
CNC 8055
CNC 8055i
OPERATING IN JOG MODE
2.
·TC· OPTION
SOFT: V02.2X
·63·
Live tool
Example of a PLC program to manage the live tool
Here is an example of the portion of the PLC program that must manage the live tool:
( ) = CNCRD (TOOL, R101, M1)
Assigns the number of the active tool to register R101.
= CNCRD (TOF R101, R102, M1)
Loads register R102 with the location code of the active tool.
CPS R102 EQ 10 OR CPS R102 EQ 20 OR CPS R102 EQ 30 = M2
If the active tool is a live tool (if its location code is 10, 20 or 30), it activates the M2 mark.
CUSTOM AND (DFU B7R561 OR DFD M2) = CNCEX1 (M45 S0, M1)
If while the TC (CUSTOM=1) mode is selected, the "Stop live tool" key is pressed (DFU B7R561)
or the live tool is de-selected (DFD M2).
The PLC "tells" the CNC to execute block M45 S0 (stops the live tool).
CUSTOM AND M2 AND DFU B3R562 = CNCRD (LIVRPM, R117, M1) = CNCWR (R117, GUP100,
M1)= CNCEX1 (M45 SP100, M1)
If in TC (CUSTOM=1) mode, a live tool is selected (M2) and the "live tool clockwise" key is
pressed (DFU B3R562).
The PLC reads in R117 the rpm currently selected for the live tool (LIVRPM) and assigns them
to general parameter P100.
Finally, the PLC "tells" the CNC to execute block M45 SP100 (live tool clockwise at the selected
rpm).
CUSTOM AND M2 AND DFU B5R562 = CNCRD (LIVRPM, R117, M1) = CNCWR (R117, GUP100,
M1)= CNCEX1 (M45 S-P100, M1)
If in TC (CUSTOM=1) mode, a live tool is selected (M2) and the "live tool counterclockwise" key
is pressed (DFU B5R562).
The PLC reads in R117 the rpm currently selected for the live tool (LIVRPM) and assigns them
to general parameter P100.
Finally, the PLC "tells" the CNC to execute block M45 S-P100 (live tool counterclockwise at the
selected rpm).
Page 64
·64·
Operating manual
CNC 8055
CNC 8055i
2.
OPERATING IN JOG MODE
·TC· OPTION
SOFT: V02.2X
Spindle control
2.9 Spindle control
The standard screen of the TC mode has a window that shows the following spindle related data.
Since it is possible to work with the spindle in rpm, at CSS or in orientation mode, the information
shown by that window will be different in each case.
To switch from one mode to the other, press the key:
On CNC power-up and after the keystroke sequence [SHIFT] [RESET], the CNC selects the rpm
mode. When working at constant surface speed (CSS), the light of the [CSS] key is on.
S 0100
% 115
SMAX 1000
RANGE 1
CSS 0100
% 115
SMAX 1000
RANGE 1
S 0100
% 115
SMAX 1000
RANGE 1
S 0100
% 115
SMAX 1000 RANGE 1
020.0000
CSS rpm without
spindle
orientation
rpm with
spindle
orientation
CSS
m / min
CSS
m / min
Page 65
Operating manual
CNC 8055
CNC 8055i
OPERATING IN JOG MODE
2.
·TC· OPTION
SOFT: V02.2X
·65·
Spindle control
2.9.1 Spindle in rpm
The CNC displays the following information.
1. Real spindle speed in rpm.
2. Theoretical spindle speed in rpm.
To select another speed, press the [S] key. The CNC highlights the current value.
Enter the new value and press [START]. The CNC assumes that value and refreshes the real
spindle speed.
3. Spindle status.
To modify the spindle status, press the following keys:
4. Percentage of the theoretical spindle speed being applied.
To modify the percentage (%), press the following keys.
5. Maximum spindle speed in rpm.
To select another speed, press the [S] key twice. The CNC highlights the current value. Enter
the new value and press [ENTER]. The CNC assumes this value and does not allow the spindle
to exceed these rpm.
The maximum spindle speed is saved in the MDISL variable. This variable is updated (refreshed)
changing the SMAX value and when programming function "G92 S" via ISO.
Spindle clockwise
Spindle counterclockwise
Outside rounding
15:28:42 SBK P000002 IN POSITION
X
Z
S
00044.000
-00443.331
115
HOME X 0000.000
HOME Z 0000.000
F 0100.000
% 080
T 02
S 0100
D 12
CHANGE POSITION
X 25.000 Z 85.000
% 115
SMAX 1000
RANGE 1
1
2
3 4
5
6
SPINDLE
SPEED
%
+
-
%+
%-
SPINDLE
SPEED
%
+
-
Page 66
·66·
Operating manual
CNC 8055
CNC 8055i
2.
OPERATING IN JOG MODE
·TC· OPTION
SOFT: V02.2X
Spindle control
6. Spindle gear currently selected.
This value cannot be changed when using an automatic gear change.
When not using an automatic tool changer, press the [S] key and then use the [] key to highlight
the current value. Enter the gear number to be selected and press [ENTER] or [START].
When the machine does not use spindle gears, this message makes no sense. That is why the CNC
does not show this message when text 28 of program 999997 has not been defined.
i
Page 67
Operating manual
CNC 8055
CNC 8055i
OPERATING IN JOG MODE
2.
·TC· OPTION
SOFT: V02.2X
·67·
Spindle control
2.9.2 Spindle in constant surface speed mode
In constant surface speed mode, the user sets the tangential speed that must always be kept
between the tool tip and the part. Therefore, the spindle rpm depend on the position of the tool tip
with respect to the rotation axis. Thus, if the tool tip gets away from the rotation axis, the spindle
slows down and if it gets closer, it speeds up.
The CNC displays the following information.
1. Real spindle speed in rpm.
2. Theoretical constant surface speed. This speed is defined in meters/min or feet/min.
To select another speed, press the [S] key. The CNC highlights the current value.
Enter the new value and press [START]. The CNC assumes this value and if the spindle is
turning, it updates the real spindle speed.
3. Spindle status.
To modify the spindle status, press the following keys:
4. Percentage of the theoretical spindle speed being applied.
To modify the percentage (%), press the following keys.
Spindle clockwise
Spindle counterclockwise
Outside rounding
15:28:42 SBK P000002 IN POSITION
X
Z
S
00044.000
-00443.331
115
HOME X 0000.000
HOME Z 0000.000
F 0100.000
% 080
T 02
CSS 0100
D 12
CHANGE POSITION
X 25.000 Z 85.000
% 115
SMAX 1000
RANGE 1
1
2
3 4
5
6
SPINDLE
SPEED
%
+
-
%+
%-
SPINDLE
SPEED
%
+
-
Page 68
·68·
Operating manual
CNC 8055
CNC 8055i
2.
OPERATING IN JOG MODE
·TC· OPTION
SOFT: V02.2X
Spindle control
5. Maximum spindle speed in rpm.
To select another speed, press the [S] key twice. The CNC highlights the current value. Enter
the new value and press [ENTER]. The CNC assumes this value and does not allow the spindle
to exceed these rpm.
The maximum spindle speed is saved in the MDISL variable. This variable is updated (refreshed)
changing the SMAX value and when programming function "G92 S" via ISO.
6. Spindle gear currently selected.
This value cannot be changed when using an automatic gear change.
When not using an automatic tool changer, press the [S] key and then use the [] key to highlight
the current value. Enter the gear number to be selected and press [ENTER] or [START].
Working at constant surface speed mode
When selecting the constant surface speed mode, the CNC assumes the spindle gear (range) that
is currently selected. The following cases may occur in this mode, when selecting a new constant
surface speed value:
• The spindle is stopped.
The CNC selects the new speed, but it does not apply it until the starts turning.
• The spindle is running.
The CNC, depending on the position of the axis, calculates and turns the spindle at the
corresponding rpm so the constant surface speed is the one defined.
The following cases may occur when moving the axes when working at constant surface speed:
• The spindle is running.
The CNC moves the axes at the programmed F.
As the X axis moves, the CNC adapts the spindle speed (rpm) to maintain the selected constant
speed. Thus, if the tool tip gets away from the rotation axis, the spindle slows down and if it gets
closer, it speeds up.
The CNC limits the spindle rpm to the maximum speed set by "SMAX".
• The spindle is stopped, but a spindle speed S has been selected.
The CNC calculates the feedrate F in mm/min for the last programmed S and moves the axis.
For example if «F 2.000» and «S 500»:
Feedrate = F (mm/rev) x S (rev/min) = 2 x 500 = 1000 mm/min.
The axis moves at a feedrate of 1000 mm/min.
• The spindle is stopped and no spindle speed S has been selected.
If F = 0, the CNC moves the axes in rapid.
When the machine does not use spindle gears, this message makes no sense. That is why the CNC
does not show this message when text 28 of program 999997 has not been defined.
i
If F is other than 0, the axes can only be moved by pressing the rapid key and an axis
key. The CNC moves the axis in rapid.
Page 69
Operating manual
CNC 8055
CNC 8055i
OPERATING IN JOG MODE
2.
·TC· OPTION
SOFT: V02.2X
·69·
Spindle control
2.9.3 Spindle orientation
When using spindle orientation (general machine parameter REFEED1 (P34) other than 0), the
CNC shows the following information.
1. Real spindle speed in rpm.
2. Spindle angular position in degrees.
This information is shown when working in spindle orientation mode. When switching to RPM
mode, it only shows the actual (real) spindle speed.
3. Theoretical spindle speed in rpm.
To select another speed, press the [S] key. The CNC highlights the current value.
Enter the new value and press [START]. The CNC assumes that value and refreshes the real
spindle speed.
4. Spindle status.
When working in spindle orientation mode, it always shows the "spindle stopped" symbol.
5. Percentage of the theoretical spindle speed being applied.
The CNC does not apply this factor when working in spindle orientation mode. It only applies
it when working in RPM mode.
To modify the percentage (%), press the following keys.
6. Maximum spindle speed in rpm.
To select another speed, press the [S] key twice. The CNC highlights the current value. Enter
the new value and press [ENTER]. The CNC assumes this value and does not allow the spindle
to exceed these rpm.
The maximum spindle speed is saved in the MDISL variable. This variable is updated (refreshed)
changing the SMAX value and when programming function "G92 S" via ISO.
Spindle clockwise
Spindle counterclockwise
Outside rounding
6 7
15:28:42 SBK P000002 IN POSITION
X
Z
S
00044.000
-00443.331
115
HOME X 0000.000
HOME Z 0000.000
F 0100.000
% 080
T 02
S 0100
D 12
CHANGE POSITION
X 25.000 Z 85.000
% 115
SMAX 1000 RANGE 1
S pos 80.000
1
3
4 5
8
2
020.0000
%+
%-
SPINDLE
SPEED
%
+
-
Page 70
·70·
Operating manual
CNC 8055
CNC 8055i
2.
OPERATING IN JOG MODE
·TC· OPTION
SOFT: V02.2X
Spindle control
7. Spindle gear currently selected.
To select another gear, when not using an automatic tool changer, press the [S] key and then
use the [] key until the current value is highlighted.
Enter the gear number to be selected and press [ENTER] or [START].
8. Spindle angular increment when working in spindle orientation mode.
To select another value, press the [S] key three times. The CNC highlights the current value.
Enter the new value and press [ENTER].
Working with spindle orientation
When having spindle orientation, the CNC uses the same screen when working in RPM mode and
when working in spindle orientation mode.
RPM mode.
Press one of these three keys to select this mode. The screen will not show the angular position
of the spindle.
Spindle orientation mode
Press the key for spindle orientation to select this mode:
The spindle will stop (if it was turning), it then searches home and finally positions at the angular
position indicated on the lower right side of the screen (at 20º in the upper figure).
Every time the spindle orientation key is pressed, the spindle position increments in that value (20º
in the upper figure).
When the machine does not use spindle gears, this message makes no sense. That is why the CNC
does not show this message when text 28 of program 999997 has not been defined.
i
15:28:42 SBK P000002 IN POSITION
X
Z
S
00044.000
-00443.331
115
HOME X 0000.000
HOME Z 0000.000
F 0100.000
% 080
T 02
S 0100
D 12
CHANGE POSITION
X 25.000 Z 85.000
% 115
SMAX 1000 RANGE 1
S pos 80.000
020.0000
SPINDLE
SPEED
%
+
-
Page 71
Operating manual
CNC 8055
CNC 8055i
OPERATING IN JOG MODE
2.
·TC· OPTION
SOFT: V02.2X
·71·
Controlling the external devices
2.10 Controlling the external devices
With this CNC, it is possible to activate and deactivate, via keyboard, up to 6 external devices, for
example, the coolant.
The machine manufacturer must use the PLC program to activate and deactivate the devices. The
CNC will inform the PLC about the status of each key. The corresponding register bit will be set to
1 when the key is pressed and 0 when it is not pressed.
The register bit for each key is:
The status of the lamp of each key must be controlled by the machine manufacturer through the
PLC program using the input variables TCLED* indicated in the figure.
Examples:
Coolant control:
DFU B28R561 = CPL TCLED1 = CPL O33
Tailstock control (O1). A number of conditions must be met for activating or deactivating the
tailstock, such as spindle stopped, etc.
DFU B30R561 AND (Rest of conditions) = CPL TCLED2 = CPL O34
O2 O4
O5O3O1
B30
R561
B28
R561
B29
R561
B31
R561
B2
R562
B4
R562
TCLED1
(M5032)
TCLED3
(M5034)
TCLED5
(M5036)
TCLED2
(M5033)
TCLED4
(M5035)
TCLED6
(M5037)
Page 72
·72·
Operating manual
CNC 8055
CNC 8055i
2.
OPERATING IN JOG MODE
·TC· OPTION
SOFT: V02.2X
ISO management
2.11 ISO management
Access to the MDI mode or the ISO mode.
The ISO key may be used to access the MDI mode or the ISO mode.
To access the MDI mode, the CNC must be in jog mode and the ISO key must be pressed. The CNC
will show a window at the bottom of the standard (or special) screen.
In this window, it is possible to edit a block in ISO code and then execute it, like in MDI in T mode.
Displaying the last 10 MDI instructions.
From the MDI mode, pressing the [UP ARROW] or [DOWN ARROW] key opens a window that shows
the last 10 instructions that have been executed. This window resizes itself to fit the number of
instructions that have been saved.
To execute or modify an MDI line that has been executed earlier, proceed as follows:
• Go into MDI mode.
• Press the [UP ARROW] or [DOWN ARROW] key to open the window that shows the last MDI
instructions (up to 10).
• Use the [UP ARROW] or [DOWN ARROW] key to select the desired instruction.
Press [START] to execute the selected instruction.
Press [ENTER] to modify the selected instruction. Once the instruction has been modified,
press [START] to execute it.
Considerations:
• An MDI instruction is saved only if it is correct and if it is not the same as the previous one on
the list.
• The instructions are kept saved even after turning the unit off.
ISO
ISO
15:28:42
X
Z
S
00044.000
-00443.331
115
HOME X 0000.000
HOME Z 0000.000
F 0100.000
% 080
T 02
S 0100
D 12
CHANGE PO SITION
X 25.000 Z 85.000
% 115
SMAX 1000
P000002
15:28:42
M0
(MSG " " )
(IF P102 EQ 1 GOTO N10)
(IF P101 EQ 0 RET)
M3
(RET)
N10 M4
(RET)
G01 G18
M41
PARTC : 000000
CYTIME : 00:00:00:00
TIMER: : 000000:00:00
COMMAND
X 00000.000
Z 00000.000
THEORETICAL
ACTUAL
X 00000.000
Z 00000.000
RPM M/MIN
TO GO
X 00000.000
Z 00000.000
X 00000.000
Z 00000.000
FOLLOWING ERROR
S 0.0000 S 0.000 0 S 0.0000 S 0. 0000
P000002
Page 73
Operating manual
CNC 8055
CNC 8055i
OPERATING IN JOG MODE
2.
·TC· OPTION
SOFT: V02.2X
·73·
ISO management
Generating an ISO-coded program
In the conversational mode of the CNC, it is possible to generate an ISO-coded program from an
operation (cycle) or on a part-program. See "7.5 Graphic representation" on page 203.
Page 74
·74·
Operating manual
CNC 8055
CNC 8055i
2.
OPERATING IN JOG MODE
·TC· OPTION
SOFT: V02.2X
ISO management
Page 75
CNC 8055
CNC 8055i
·TC· OPTION
SOFT: V02.2X
3
·75·
WORKING WITH OPERATIONS OR
CYCLES
Use the following CNC keys to select the different machining operations or cycles.
User cycles
The user cycle is edited like any other standard cycle of the TC mode. Once all the required data
has been defined, the user can simulate or execute the cycle like any other standard cycle of the
TC mode.
Cycles or operations of the CNC
When pressing any other key, the CNC selects the corresponding standard machining cycle,
changes the display and turns on the lamp of the key that has been pressed (indicating the selected
type.
Standard machining operations or cycles may be selected with each one of the following keys:
It is possible to combine ISO-coded blocks with standard and/or user cycles to create par t-programs.
Chapter "6 Saving programs"describes in detail how to do it and how to use those programs.
To de-select a cycle and return to the standard screen, press the key for the selected cycle (the one
with the lamp on) or the [ESC] key.
When pressing [PCALL], the CNC shows all the user cycles defined by the machine
manufacturer with the WGDRAW application.
Positioning cycle. Threading cycle.
Turning cycle. Grooving cycle.
Facing cycle. Drilling and tapping cycle.
Taper turning cycle. Profiling cycle.
Rounding cycle.
When the machining operation or cycle has several levels, [LEVEL CYCLE] must be
pressed to select the desired cycle level.
PCALL
FAGOR
PCALL
PCALL
LEVEL
CYCLE
Page 76
·76·
Operating manual
CNC 8055
CNC 8055i
3.
WORKING WITH OPERATIONS OR CYCLES
·TC· OPTION
SOFT: V02.2X
When operating in conversational mode, do not use global parameters 150 through 299 (both
included), because the operations or cycles can modify these parameters and cause the machine to
malfunction.
Page 77
Operating manual
CNC 8055
CNC 8055i
WORKING WITH OPERATIONS OR CYCLES
3.
·TC· OPTION
SOFT: V02.2X
·77·
Operation editing mode
3.1 Operation editing mode
Once the operation has been selected, the CNC shows a screen like the following:
1. Name of the selected operation or work cycle.
2. Help graphics.
3. Spindle conditions to execute the cycle.
4. Current machine status. Coordinates and machining conditions.
5. Data defining the machining geometry.
6. Machining conditions for the roughing operation.
7. Machining conditions for the finishing operation.
The CNC will highlight an icon, a coordinate or one of the data defining the operation or cycle
indicating that it has been selected. Use the following keys to select another icon, data or coordinate.
The coordinates for the X axis are defined in the work units, radius or diameter. Later on, each
operation or cycle indicates the units used to define the data associated with the X axis (safety
distance, pass, excess stock, etc.).
The CNC selects the previous one or the next one.
The CNC selects the first coordinate for that axis. Pressing that key again
selects the next coordinate for that axis.
The CNC selects the corresponding roughing data. Pressing that key again
selects the corresponding finishing data.
The CNC selects the "S" roughing data. Pressing that key again selects the
finishing "S" data and pressing it again selects the data for the spindle SMAX.
15:28:42
Coordinate (Xi, Zi)
X 0.0000 Z 0.0000
Z
X
Xf, Zf
Xi, Zi
Coordinate (Xf, Zf)
X 0.0000 Z 0.0000
TURNING CYCLE
Diameter
0.0000
Safety distance
X 0.0000 Z 0.0000
X 00044.000 Z -00397.490
F 1.000 S 150 T 3
F 0.000 S 150 T 3
ROUGHING
0
F 0.000 S 150 T 3
FINISHING
z 0
x 0
RPM
GEAR
SMAX 1230
2
1
2
3
4
5
6
7
>
/<][
X
AR
EY
Z
J"
F
Q!
T
NÑ
S
Page 78
·78·
Operating manual
CNC 8055
CNC 8055i
3.
WORKING WITH OPERATIONS OR CYCLES
·TC· OPTION
SOFT: V02.2X
Operation editing mode
3.1.1 Definition of spindle conditions
Work mode (RPM) or (CSS)
Place the cursor on the "RPM" or "CSS" icon. To do this, use the [CSS] key or the [] [] [] [] keys.
Once the data has been selected, press the [CSS] key or the two-color key to change the work mode.
Spindle range
Place the cursor over this data, key in the desired value and press [ENTER].
In cycles using a live tool:
Maximum spindle speed (S) in rpm
Place the cursor over this data, key in the desired value and press [ENTER].
Spindle turning direction
There are two ways to select the spindle turning direction.
Coolant
There are two ways to turn the coolant on or off.
Once the operation or the cycle is completed or the part-program it belongs to, the CNC outputs
the M9 function to the PLC.
Icon for selecting the spindle gear to be used for machining cycles where a live tool is
used. Its possible values are:
Value 0: Gear corresponding to the S value
Value 1: Gear 1
Value 2: Gear 2
Value 3: Gear 3
Value 4: Gear 4
Place the cursor on this data and press the two-color key to change the icon.
Start the spindle in the desired direction with the JOG keys. The CNC starts the
spindle and assumes that turning direction as spindle turning data for the cycle.
Place the cursor on this data and press the two-color key to change the icon.
Turns the coolant on. The CNC outputs the M8 function to the PLC.
Turns the coolant off. The CNC outputs the M9 function to the PLC.
CSS
m / min
>
/<][
*
*
Page 79
Operating manual
CNC 8055
CNC 8055i
WORKING WITH OPERATIONS OR CYCLES
3.
·TC· OPTION
SOFT: V02.2X
·79·
Operation editing mode
3.1.2 Definition of machining conditions
Some operations keep the machining conditions throughout the execution (positioning cycles,
drilling cycle, etc.). Other operations use some machining conditions for roughing and others for
finishing (turning cycle, rounding cycle, etc.).
This section describes how to define all this data.
Selecting the roughing operation.
Place the cursor on the roughing checkbox, select or de-select the roughing operation pressing the
[TWO-COLOR] key and press [ENTER]. When de-selecting the roughing, all its data will stay in gray.
The data "side finishing stock" of the finishing portion is turned on/off using the roughing checkbox
Selecting the finishing operation.
Place the cursor on the finishing checkbox, select or de-select the finishing operation pressing the
[TWO-COLOR] key and press [ENTER]. When de-selecting the finishing, all its data will stay in gray.
Axis feedrate (F).
Spindle turning speed (S).
Machining tool (T).
Place the cursor over this data, key in the desired value and press [ENTER].
The CNC updates the associated offset (D) and refreshes the associated icon showing the graphics
for the location code (shape) of the new tool.
Press [ESC] to quit the tool calibration mode and return to the cycle
Tool offset number (D).
Place the cursor over this data, key in the desired value and press [ENTER].
Place the cursor over this data, key in the desired value and press [ENTER].
Place the cursor over this data, key in the desired value and press [ENTER].
It is also possible to access the tool calibration mode to check or modify the data for the
selected tool. To do that, place the cursor on the "T" and press the key associated with
tool calibration.
Pocket machining direction.
Icon to set the machining direction of the roughing tool.
ENTER
ENTER
Page 80
·80·
Operating manual
CNC 8055
CNC 8055i
3.
WORKING WITH OPERATIONS OR CYCLES
·TC· OPTION
SOFT: V02.2X
Operation editing mode
Machining direction.
Some cycles allow the machining direction to be selected (turning direction or facing direction).
Roughing pass ().
Finishing stock (
).
Sideways penetration angle (
,
).
Sideways penetration angle. If programmed with a value smaller than or equal to 0º, or greater than
90º, it issues the corresponding error message. If not programmed, it assumes 90º.
Auxiliary "M" functions.
There is a window for setting up to 4 auxiliary M functions in the roughing and finishing operations.
The functions will be executed in the same order as these are arranged on the list.
Select the corresponding window with the [][] keys Use the [][] keys to move around the
window.
To delete a function, select it and press [CLEAR]
Place the cursor on this icon and press the two-color key. The icon changes and the help
graphics are refreshed.
Place the cursor over this data, key in the desired value and press [ENTER]. The roughing
pass is always defined in radius.
The roughing pass is always defined in radius. Place the cursor over this data, key in the
desired value and press [ENTER].
Z
X
Xi, Zi
1
2
5
3
4
Z
X
Xi, Zi
1
25
3
4
Turning direction. Facing direction.
*
ENTER
ENTER
The availability of "M" functions in the cycles is determined with g.m.p. "CODISET (P147)".
i
Page 81
Operating manual
CNC 8055
CNC 8055i
WORKING WITH OPERATIONS OR CYCLES
3.
·TC· OPTION
SOFT: V02.2X
·81·
Operation editing mode
3.1.3 Cycle level
All the cycles have several editing levels. Each level has its own screen and the main window of the
cycle indicates, with tabs, the available levels and which one is selected.
To change levels, use the [LEVEL CYCLE] key or the [page up] and [page down] keys
to scroll up and down through the various levels.
15:28:42
Coordinate (Zf)
Z 0.0000
Z
X
Zf
Xi, Zi
H
P
Safety distance
X 0.0000 Z 0.0000
Thread pitch
P 0.0000
Distance t o end of thread
0.0000
Total depth
H 0.0000
Coordinate (Xi, Zi)
X 0.0000 Z 0.0000
THREADING CYCLE 1
X 00044.000 Z -00397.490
F 1.000 S 150 T 3
S 150 T 2 0
F 0.0200
Minimum increment
SMAX 0
RPM
Max. pass of depth
1
1
LEVEL
CYCLE
Page 82
·82·
Operating manual
CNC 8055
CNC 8055i
3.
WORKING WITH OPERATIONS OR CYCLES
·TC· OPTION
SOFT: V02.2X
Simulating and executing the operation
3.2 Simulating and executing the operation
All the operations or cycles have 2 work modes; execution and editing.
• Press [ESC] to switch from editing mode to execution mode.
• Press [ESC] to switch from executing mode to editing mode.
For further information on simulating and executing cycles, see the chapter "7 Execution and
simulation".
The operation or cycle may be simulated in either mode. To do that, press the
[GRAPHICS] key.
To execute the operation or cycle, select the execution mode and press [START].
>
/<][
X
AR
EY
Z
J"
F
NÑ
S
Q!
T
Editing mode Execution mode
15:28:42
Coordinate (Xi, Zi)
X 0.0000 Z 0.0000
Z
X
Xf, Zf
Xi, Zi
Coordinate (Xf, Zf)
X 0.0000 Z 0.0000
Diameter
0.0000
Safety distance
X 0.0000 Z 0.0000
TURNING CYCLE 1
X 00044.000 Z -00397.490
F 1.000 S 150 T 3
F 0.000 S 150 T 3
ROUGHING ROUGHING PASS
0
F 0.000 S 150 T 3
FINISHING FINISHIN G STOCK
0
RPM
GEAR
SMAX 1230
2
15:28:42
Coordinate (Xi, Zi)
X 0.0000 Z 0.0000
Z
X
Xf, Zf
Xi, Zi
Coordinate (Xf, Zf)
X 0.0000 Z 0.0000
Diameter
0.0000
Safety distance
X 0.0000 Z 0.0000
TURNING CYCLE 1
F 0.000 S 150 T 3
ROUGHING ROUGHING PASS
0
F 0.000 S 150 T 3
FINISHING FINISHING ST OCK
0
RPM
GEAR
SMAX 1230
2
GRAPHICS
Page 83
Operating manual
CNC 8055
CNC 8055i
WORKING WITH OPERATIONS OR CYCLES
3.
·TC· OPTION
SOFT: V02.2X
·83·
Simulating and executing the operation
3.2.1 Background cycle editing
It is possible to edit an operation or cycle while executing a program or part (background editing).
The new operation edited may be saved as part of a part-program other than the one being executed.
The operation being edited in background cannot be executed or simulated, and the current position
of the machine cannot be assigned to a coordinate.
Use the following keys to inspect or change a tool while editing in background.
Pressing the [T] key without quitting background editing selects the T field of the operation or of the
canned cycle being edited.
Interrupts the execution and goes on editing in background.
To quit background editing.
To access tool inspection.
ESC
Q!
T
Background editing is not possible while executing an independent operation or cycle. It can only be
done while executing a program or part.
i
Page 84
·84·
Operating manual
CNC 8055
CNC 8055i
3.
WORKING WITH OPERATIONS OR CYCLES
·TC· OPTION
SOFT: V02.2X
Positioning cycle
3.3 Positioning cycle
Level 1.
The following data must be defined:
• Coordinates of the target point.
• How the movement is to be carried out.
• The type of feed; in rapid or at the programming feedrate.
Level 2.
The following data must be defined:
• Coordinates of the target point.
• How the movement is to be carried out.
• The type of feed; in rapid or at the programming feedrate.
• The auxiliary functions that will be executed before and after the movement.
This key accesses the positioning operation.
This cycle may be defined in two ways:
Z
X
X, Z
Page 85
Operating manual
CNC 8055
CNC 8055i
WORKING WITH OPERATIONS OR CYCLES
3.
·TC· OPTION
SOFT: V02.2X
·85·
Positioning cycle
3.3.1 Definition of data
Order in which the axes move.
Type of feedrate.
Coordinates of the target point (X, Z).
The coordinates are defined one by one. After placing the cursor on the coordinates of the axes to
be defined, the value is entered in one of the following ways.
• Entering the value manually. Key in the desired value and press [ENTER].
• Assign the current machine position.
Jog the axis with the handwheel or the JOG keys up to the desired point. Press [RECALL] so
the selected data assumes the value shown in the top right window and press [ENTER].
The top right window shows the tool position at all times.
Auxiliary "M" functions.
Auxiliary function “M” is the name given to the functions determined by the manufacturer which allow
the different machine devices to be governed. Some auxiliary "M" functions are used to interrupt
the program, to select the spindle turning direction, to control the coolant, the spindle gear box, etc.
The programming manual describes how to program these functions and the installation manual
describes how to set up the system to use them.
To define the auxiliary functions, select the corresponding window with the [][] keys. Use the
[][] keys to move around the window. To delete a function, select it and press [CLEAR]
The functions will be executed in the same order as these are arranged on the list.
To select the moving order, place the cursor over this icon and press the two-color key.
All two axes at the same time.
First X and then Z.
First Z and then X.
To select the type of feedrate, place the cursor over this icon and press the two-color key.
Programmed feedrate.
Rapid feed.
*
X-Z
Z-X
Z
X
X, Z
Z
X
X, Z
X-Z
Z
X
X, Z
Z-X
*
Page 86
·86·
Operating manual
CNC 8055
CNC 8055i
3.
WORKING WITH OPERATIONS OR CYCLES
·TC· OPTION
SOFT: V02.2X
Turning cycle
3.4 Turning cycle
Turning levels 1 and 2
Level 1.
The following data must be defined:
• Coordinates of the starting point.
• Coordinates of the last point.
• The final diameter.
• The safety distance.
Level 2.
The following data must be defined:
• Coordinates of the starting point.
• Coordinates of the last point.
• The final diameter.
• The type of machining at each corner.
• The safety distance.
This key accesses the turning cycle.
This cycle may be defined in several ways:
Z
X
Xf, Zf
Xi, Zi
Page 87
Operating manual
CNC 8055
CNC 8055i
WORKING WITH OPERATIONS OR CYCLES
3.
·TC· OPTION
SOFT: V02.2X
·87·
Turning cycle
Turning levels 3, 4 and 5
Level 3. Rectangular pocket on the cylindrical side of the part.
Level 4. Circular pocket on the cylindrical side of the part.
ZC plane
YZ plane
ZC plane
YZ plane
Page 88
·88·
Operating manual
CNC 8055
CNC 8055i
3.
WORKING WITH OPERATIONS OR CYCLES
·TC· OPTION
SOFT: V02.2X
Turning cycle
Level 5. ZC / YZ profile pocket.
Y
Z
x
Fx
I
P
Dx
x
Fx
I
P
Dx
C
Z
Front view
Y axis
"C" axis
Front view
Page 89
Operating manual
CNC 8055
CNC 8055i
WORKING WITH OPERATIONS OR CYCLES
3.
·TC· OPTION
SOFT: V02.2X
·89·
Turning cycle
3.4.1 Data definition (levels 1 and 2)
Type of turning operation.
When changing the type of turning operation, the CNC changes the icon and shows the
corresponding help screen.
Coordinates of the first point (Xi, Zi) and of the last point (Xf, Zf).
The coordinates are defined one by one. After placing the cursor on the coordinates of the axes to
be defined, the value is entered in one of the following ways.
• Entering the value manually. Key in the desired value and press [ENTER].
• Assign the current machine position.
Jog the axis with the handwheel or the JOG keys up to the desired point. Press [RECALL] so
the selected data assumes the value shown in the top right window and press [ENTER].
The top right window shows the tool position at all times.
Final diameter ().
Place the cursor over this data, key in the desired value and press [ENTER].
Safety distance.
In order to prevent collisions with the part, the CNC allows a part approach point to be set. The safety
distance indicates the position of the approach point referred to the starting point (Xi, Zi).
To change one of these values, place the cursor on the corresponding data, key in the desired value
and press [ENTER].
The value of the safety distance on X is always defined in radius.
To select the type of turning operation, place the cursor over this icon and press the twocolor key.
Inside turning.
Outside turning.
*
Z
X
Xi, Zi
X
Z
Page 90
·90·
Operating manual
CNC 8055
CNC 8055i
3.
WORKING WITH OPERATIONS OR CYCLES
·TC· OPTION
SOFT: V02.2X
Turning cycle
Type of machining to be carried out on each corner.
For a rounded corner, define the rounding radius (R); for a chamfer, define the distance from the
theoretical corner to the chamfer point (C).
Finishing stocks in X-Z.
2 different residual stocks may be defined, one for each axis (X, Z). To define these residual stocks,
place the cursor on the corresponding data, key in the desired value and press [ENTER].
To select the type of corner, place the cursor over this icon and press the two-color key.
*
R
R
C
C
C
Square corner. Rounded corner. Chamfered corner.
Page 91
Operating manual
CNC 8055
CNC 8055i
WORKING WITH OPERATIONS OR CYCLES
3.
·TC· OPTION
SOFT: V02.2X
·91·
Turning cycle
3.4.2 Data definition (levels 3, 4 and 5)
Level 3:
Level 4:
Icon for selecting the ZC or YZ plane.
Icon to select the position of the starting point.
Z,C / Z,Y: Coordinates of the starting point.
L, H: Pocket dimensions.
: Inclination angle of the rectangular pocket.
W: Angular position of the spindle (in degrees) where the pocket will be milled in the YZ
plane.
Icon for selecting the vertex type in the pocket corners:
•Normal vertix
• Rounded vertix
• Chamfered vertix
r / c: Value of the corner rounding or chamfering radius in the rectangular pocket.
Dx: Safety distance on the longitudinal axis (cylindrical side).
Dz: Safety distance on the longitudinal axis (face).
X: Part plane.
P: Total rectangular pocket depth. When programmed with a 0 value, it generates the
corresponding error.
I: Penetration step (pass) when roughing:
• If programmed with a positive value, the actual step (pass) will be the one closest
to this value so all passes will be identical.
• If programmed with a negative value, the actual pass will be the one programmed
and the last pass will be adjusted to the final (remaining) depth.
• If not programmed, it assumes 0.
Fx: Penetration feedrate for roughing and finishing. If not programmed, it assumes 0.
Icon to select the ZC or YZ plane.
Zc, Cc /
Zc, Yc:
Center coordinates of the circular pocket.
Rc: Circular pocket radius.
W: Angular position of the spindle (in degrees) where the pocket will be milled in the YZ
plane.
Dx: Safety distance on the longitudinal axis (cylindrical side).
Dz: Safety distance on the longitudinal axis (face).
R / X: • Cylinder radius when it is the ZC plane.
• X coordinate of the part surface when it is the ZY plane.
P: Total circular pocket depth. When programmed with a 0 value, it generates the
corresponding error.
Page 92
·92·
Operating manual
CNC 8055
CNC 8055i
3.
WORKING WITH OPERATIONS OR CYCLES
·TC· OPTION
SOFT: V02.2X
Turning cycle
Level 5:
I: Penetration step (pass) when roughing:
• If programmed with a positive value, the actual step (pass) will be the one closest
to this value and all the passes will be identical.
• If programmed with a negative value, the actual pass will be the one programmed
and the last pass will be adjusted to the final (remaining) depth.
• If not programmed, it assumes 0.
Fx: Penetration feedrate for roughing and finishing. If not programmed, it assumes F/2.
Icon for selecting the machining plane (ZC plane or YZ plane).
Profile program : Number of the part-program where the pocket is defined.
Dx: Safety distance on the longitudinal axis.
X: X coordinate of the part surface when it is the YZ plane.
R: Part radius when it is the ZC plane.
P: Total profile pocket depth. If not programmed or programmed with a 0 value,
the CNC will display the corresponding error message.
I: Maximum roughing pass. If not programmed or if programmed with a 0
value, it assumes the value of 75% of the diameter of the roughing tool.
Fx: Machining feedrate on the X axis: if not programmed or programmed with
a 0 value, the CNC assumes the roughing F value for the penetration in
roughing and the finishing F for the penetration in finishing.
W: Angular position of the spindle (in degrees) where the profile will be
machined in the YZ plane (in degrees).
Spindle turning direction
Page 93
Operating manual
CNC 8055
CNC 8055i
WORKING WITH OPERATIONS OR CYCLES
3.
·TC· OPTION
SOFT: V02.2X
·93·
Turning cycle
3.4.3 Basic operation (levels 1 and 2)
The machining steps in this cycle are as follows:
1. If the roughing operation was programmed with another tool the CNC makes a tool change,
moving to the change point if the machine so requires.
2. The spindle starts with the speed selected and in the direction stated.
3. The tool approaches the starting point (Xi, Zi) in rapid, keeping the selected safety distance
according to axes X and Z.
4. Roughing operation, with successive turning passes, up to a distance from the selected final
diameter equal to the finishing stock.
This operation is carried out with the conditions set for the roughing operations; however, the
CNC calculates the actual (real) pass so all the turning passes are identical. This pass will be
equal to or under the defined value
.
Each turning pass is done as shown in the figure, starting at point "1" and after going through
points "2", "3" and "4", ending at point "5".
5. Finishing operation.
If the finishing operation has been programmed with another tool, the CNC will change the tool
and will move to the change position if so required by the machine.
The finishing of the part is carried out with the machining conditions set for finishing; feedrate
of the axes (F), spindle speed (S) and turning direction.
6. Once the operation or cycle has ended, the tool will retur n to the position it occupied when calling
the cycle; i.e. to the point where [START] was pressed.
When executing an entire part, combination of operations or cycles, the tool does not return to
that point after executing each cycle.
7. The CNC stops the spindle, but it keeps the machining conditions set for finishing; tool (T),
feedrate of the axes (F) and spindle speed (S).
Z
X
Xi, Zi
X
Z
Z
X
Xi, Zi
1
23
45
Page 94
·94·
Operating manual
CNC 8055
CNC 8055i
3.
WORKING WITH OPERATIONS OR CYCLES
·TC· OPTION
SOFT: V02.2X
Turning cycle
Considerations
How to leave out the roughing or finishing operations.
By selecting T0 as the roughing tool, the cycle does not execute the roughing operation. This means
that after approaching the finishing operation will be carried out.
By selecting T0 as the finishing tool, the cycle does not execute the finishing operation. In other
words, after the roughing operation, the tool will move to the approach point maintaining the safety
distance from the starting point (Xi, Zi).
Different Xi and Xf coordinates.
When the surface to be machined is not totally cylindrical (different Xi and Xf coordinates), the CNC
analyzes both coordinates and takes as the X coordinate of the starting point the one farthest away
from the final diameter.
Z
X
Xf, Zf
Xi, Zi
Z
X
Page 95
Operating manual
CNC 8055
CNC 8055i
WORKING WITH OPERATIONS OR CYCLES
3.
·TC· OPTION
SOFT: V02.2X
·95·
Facing cycle
3.5 Facing cycle
Facing levels 1 and 2
Level 1.
The following data must be defined:
• Coordinates of the starting point.
• Coordinates of the last point.
• The final diameter.
• The safety distance.
Level 2.
The following data must be defined:
• Coordinates of the starting point.
• Coordinates of the last point.
• The final diameter.
• The type of machining at each corner.
• The safety distance.
Facing levels 3, 4 and 5
Level 3. Rectangular pocket on the face of the part.
This key accesses the facing cycle.
This cycle may be defined in several ways:
Z
X
Xf, Zf
Xi, Zi
XC plane
Page 96
·96·
Operating manual
CNC 8055
CNC 8055i
3.
WORKING WITH OPERATIONS OR CYCLES
·TC· OPTION
SOFT: V02.2X
Facing cycle
Level 4. Circular pocket on the face of the part.
XY plane
XC plane
XY plane
Page 97
Operating manual
CNC 8055
CNC 8055i
WORKING WITH OPERATIONS OR CYCLES
3.
·TC· OPTION
SOFT: V02.2X
·97·
Facing cycle
Level 5. XC / XY profile cycle.
X
Y
Fx
P
I
z
Dz
X
C
Fx
P
I
z
Dz
Y axis
"C" axis
Side view
Side view
Page 98
·98·
Operating manual
CNC 8055
CNC 8055i
3.
WORKING WITH OPERATIONS OR CYCLES
·TC· OPTION
SOFT: V02.2X
Facing cycle
3.5.1 Data definition (levels 1 and 2)
Coordinates of the first point (Xi, Zi) and of the last point (Xf, Zf).
The coordinates are defined one by one. After placing the cursor on the coordinates of the axes to
be defined, the value is entered in one of the following ways.
• Entering the value manually. Key in the desired value and press [ENTER].
• Assign the current machine position.
Jog the axis with the handwheel or the JOG keys up to the desired point. Press [RECALL] so
the selected data assumes the value shown in the top right window and press [ENTER].
The top right window shows the tool position at all times.
Final diameter ().
Place the cursor over this data, key in the desired value and press [ENTER].
Type of machining to be carried out on each corner.
For a rounded corner, define the rounding radius (R); for a chamfer, define the distance from the
theoretical corner to the chamfer point (C).
Safety distance.
In order to prevent collisions with the part, the CNC allows a part approach point to be set. The safety
distance indicates the position of the approach point referred to the starting point (Xi, Zi).
To change one of these values, place the cursor on the corresponding data, key in the desired value
and press [ENTER].
The value of the safety distance on X is always defined in radius.
Finishing stocks in X-Z.
2 different residual stocks may be defined, one for each axis (X, Z). To define these residual stocks,
place the cursor on the corresponding data, key in the desired value and press [ENTER].
To select the type of corner, place the cursor over this icon and press the two-color key.
*
R
R
C
C
C
Square corner. Rounded corner. Chamfered corner.
Z
X
Xi, Zi
X
Z
Page 99
Operating manual
CNC 8055
CNC 8055i
WORKING WITH OPERATIONS OR CYCLES
3.
·TC· OPTION
SOFT: V02.2X
·99·
Facing cycle
3.5.2 Data definition (levels 3, 4 and 5)
Level 3:
Level 4:
Icon for selecting the ZC or YZ plane.
Icon to select the position of the starting point.
Z,C /
Z,Y:
Coordinates of the starting point.
L, H: Pocket dimensions.
: Inclination angle of the rectangular pocket.
W: Angular position of the spindle (in degrees) where the pocket will be milled in the YZ
plane.
Icon for selecting the vertex type in the pocket corners:
•Normal vertix
• Rounded vertix
• Chamfered vertix
r / c: Value of the corner rounding or chamfering radius in the rectangular pocket.
Dx: Safety distance on the longitudinal axis (cylindrical side).
Dz: Safety distance on the longitudinal axis (face).
X: Part plane.
P: Total rectangular pocket depth. When programmed with a 0 value, it generates the
corresponding error.
I: Penetration step (pass) when roughing:
• If programmed with a positive value, the actual step (pass) will be the one closest
to this value so all passes will be identical.
• If programmed with a negative value, the actual pass will be the one programmed
and the last pass will be adjusted to the final (remaining) depth.
• If not programmed, it assumes 0.
Fx: Penetration feedrate for roughing and finishing. If not programmed, it assumes 0.
Icon to select the ZC or YZ plane.
Zc, Cc /
Zc, Yc:
Center coordinates of the circular pocket.
Rc: Circular pocket radius.
W: Angular position of the spindle (in degrees) where the pocket will be milled in the YZ
plane.
Dx: Safety distance on the longitudinal axis (cylindrical side).
Dz: Safety distance on the longitudinal axis (face).
R / X: • Cylinder radius when it is the ZC plane.
• X coordinate of the part surface when it is the ZY plane.
P: Total circular pocket depth. When programmed with a 0 value, it generates the
corresponding error.
Page 100
·100·
Operating manual
CNC 8055
CNC 8055i
3.
WORKING WITH OPERATIONS OR CYCLES
·TC· OPTION
SOFT: V02.2X
Facing cycle
Level 5:
I: Penetration step (pass) when roughing:
• If programmed with a positive value, the actual step (pass) will be the one closest
to this value and all the passes will be identical.
• If programmed with a negative value, the actual pass will be the one programmed
and the last pass will be adjusted to the final (remaining) depth.
• If not programmed, it assumes 0.
Fx: Penetration feedrate for roughing and finishing. If not programmed, it assumes F/2.
Icon for selecting the machining plane (XC plane or XY plane).
Profile program : Number of the part-program where the pocket is defined.
Dz: Safety distance on the longitudinal axis.
Z: Z coordinate of the part surface.
P: Total profile pocket depth. If not programmed or programmed with a 0 value,
the CNC will display the corresponding error message.
I: Maximum roughing pass. If not programmed or if programmed with a 0
value, it assumes the value of 75% of the diameter of the roughing tool.
Fz: Machining feedrate along the Z axis. If not programmed or programmed with
a 0 value, the CNC assumes the roughing F value for the penetration in
roughing and the finishing F for the penetration in finishing.
W: Angular position of the spindle (in degrees) where the profile will be
machined in the XY plane (in degrees).
Spindle turning direction
Loading...