CNC 8070
(REF: 0706)
EXAMPLES MANUAL
(·T· MODEL)
(Ref: 0706)
Examples manual (·T· model)
All rights reserved. No part of this documentation may be copied, transcribed,
stored in a data backup system or translated into any language without Fagor
Automation's explicit consent.
The information described in this manual may be modified for technical reasons.
FAGOR AUTOMATION S. COOP. Reserves the right to modify the contents of
this manual without having to communicate such modifications.
Microsoft and Windows are registered trademarks of Microsoft Corporation USA.
The other commercial trademarks belong to their respective owners.
The content of this manual and its validity for the product described here has been
verified. Even so, involuntary errors are possible, thus no absolute match is
guaranteed. Anyway, the contents of the manual is periodically checked making
and including the necessary corrections in a future edition.
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.
Examples manual (·T· model)
CNC 8070
(REF: 0706)
i
INDEX
1. Basic concepts
1.1 Basic CNC operating concepts ..........................................................................................1
1.2 Tool setting. ........................................................................................................................3
1.3 Part zero setting .................................................................................................................5
1.4 Programming of machining conditions. ..............................................................................6
1.5 Coordinate programming ...................................................................................................7
1.5.1 Example 1: Absolute and incremental coordinates.........................................................8
1.6 Tool path programming ......................................................................................................9
1.6.1 Example 2: Arc programming "G02/G03". ....................................................................10
1.6.2 Example 3: Tangential entry/exit "G37/G38" and corner rounding (radius blend) "G36" with
tool radius compensation "G40/G41/G42".12
2. Canned cycle programming
2.1 Introduction ......................................................................................................................13
2.2 Example 4. Inside turning of curved and straight sections...............................................14
2.3 Example 5. Facing of inside curved sections and outside straight sections.....................16
2.4 Example 6. Facing of inside straight sections and outside curved sections.....................18
2.5 Example 7. Inside roughing along Z axis and outside turning of curved sections............20
2.6 Example 8. Inside turning of straight sections and outside roughing along the Z axis.....22
2.7 Example 9. Inside and outside roughing along the X axis. ..............................................24
2.8 Example 10. Inside and outside taper threading..............................................................26
2.9 Example 11. Roughing along the X axis. Outside grooving and threading. .....................28
2.10 Example 12. Outside pattern repeat. Internal grooving and threading. ...........................31
2.11 Example 13: Inside and outside roughing along the X axis. ............................................34
3. C axis programming
3.1 Introduction. .....................................................................................................................37
3.2 Example 14. Machining of a profile in the ZC plane.........................................................38
3.3 Example 15. Machining of a profile in the XC plane. .......................................................39
4. Profile editor
4.1 Introduction ......................................................................................................................41
4.2 Example 16. .....................................................................................................................42
4.3 Example 17. .....................................................................................................................43
4.4 Example 18. .....................................................................................................................44
4.5 Example 19. .....................................................................................................................45
5. User subroutines
5.1 Introduction. .....................................................................................................................47
5.2 Example 20: Global subroutine. Machining of pulleys......................................................48
5.3 Creating subroutine help files:..........................................................................................50
1
CNC 8070
(REF: 0706)
1
BASIC CONCEPTS
1.1 Basic CNC operating concepts
Useful keys
Open a program.
1. Press the panel key (a).
2. Press the OPEN PROGRAM softkey [F1].
3. Use the file managing window to enter the name, number or letters of the exercise
and press [ENTER] to confirm it.
4. Once inside the program, start entering the data.
Configuring a form
• A form is the screen displayed at the CNC when editing a canned cycle.
• Press the corresponding softkey to access any form, if it is not displayed, use the
[+] softkey or press [F7],
• To access the "CYCLE EDITOR", press the corresponding key and select the
relevant cycle. Once the form has been filled out, insert it into the program.
• The forms are basically divided into three blocks: Geometry, Roughing and
Finishing.
Geometry. This block indicates the position where the cycle will be executed as
well as its dimensions.
Roughing. Machining conditions for roughing (pass, feedrate, rpm, etc.).
Finishing. Machining conditions for finishing (pass, feedrate, rpm, etc.).
• All the values entered must be confirmed with [ENTER].
(a)
Key for editing and simulation
(b)
Cycle-start button.
(c)
Reset button.
(d)
Execution button.
(e)
Cycle stop.
Examples manual (·T· model)
CNC 8070
1.
BASIC CONCEPTS
Basic CNC operating concepts
(REF: 0706)
2
Program display
There are five options when simulating a program and they may be selected
alternately with the (a) key.
1. Program test without graphic representation, it will only display the data blocks
that make up the program.
2. Solid graphics simulation. It simulates the part as a block that is previously defined
by the user.
3. Program test without graphic display, but indicating the various functions, cycles
and total execution time.
4. Simulation and program test. The screen is split in two with the program on the
left and the solid block on the right.
5. Exactly identical to the previous one, but this type of simulation does not allow
modifying any program block.
All the previous simulation options allow selecting the graphic display of the program:
Lines, combined and solid.
Syntax check
The CNC checks the syntax of each program block as it is being edited; when it
detects a mistake, it displays a line at the bottom of the screen indicating the mistake.
Program simulation.
The program must be opened prior to being simulated. Once the chosen program
appears on the screen, use the (a) key to select the simulation mode as described
in the previous section.
Machining a program.
Before executing any program, it should be simulated first to check that that it may
be machined properly.
Use the (d) key to choose the best screen type and then proceed like when simulating;
in other words, press the execution "START" key (b) to start machining. Use the
execution "STOP" key (e) to interrupt the execution of the program at any time.
The entire program can also be checked. To do that, press the vertical softkey for
syntax check. The errors found will be indicated like with the other method.
To start the simulation, press the vertical "START" simulation softkey; if an error
message appears, it will be deleted with the vertical "RESET" softkey.
Examples manual (·T· model)
CNC 8070
BASIC CONCEPTS
Tool setting.
1.
(REF: 0706)
3
1.2 Tool setting.
Tool calibration
If the CNC loses the position of the origin (for example, because the machine has
been turned off), the system must be synchronized by doing a home search before
calibrating the tools.
Home search
There are three ways to do it.
• Manually, the axes are homed one by one.
The CNC does not keep the part zero and the coordinates are displayed
referred to machine reference zero.
• Automatically, only available if the machine manufacturer has defined a homing
subroutine; all the axes are homed at the same time.
The CNC keeps the part zero and the coordinates are displayed according
to the active reference system.
Keystroke sequence to home the axes manually and automatically:
• In the program, use function G74 followed by the axes to be homed and the
number indicating their homing order.
"G74 X2 Z1 A3"
Tool calibration
There are several tool calibrating methods, either manually with a probe using a part
of known dimensions or using tool calibration canned cycles (ISO and
conversational).
To choose the one best suited for each case, refer to the manuals "Working with a
probe (·T· model) and "Operating manual" chapter 5 "Jog mode. Tool calibration"
After accessing the tool and tool magazine mode with this key, the procedure is as
follows:
1. Press [F1] to access the tool table.
• On the tool list, add the necessary tool number using [10].
• Assign to each tool all the known values and validate them using [F9] and
[ENTER].
2. Press [F4] to access the tool table of the first magazine, [F5] for the second one
and so forth.
• load the tools into the magazine one by one with [F10] or all at once pressing
[F8], [F8], [F9] [ENTER].
3. Press [F2] to access the active tool table.
• Enter the number of the tool to be calibrated and press [ENTER].
4. Calibrate the tool using the most appropriate method.
Select the axis to be homed (only manually).
Press the homing key [ZERO].
Press [START] to carry out a home search.
Examples manual (·T· model)
CNC 8070
1.
BASIC CONCEPTS
Tool setting.
(REF: 0706)
4
List of tools used in the examples:
Tool Geometry Data Tool Geometry Data
T2 T3
D:
F:
A:
B:
C:
Lc:
Rp:
1
3
60
o
7 mm.
100
o
6 mm.
0.4 mm.
D:
F:
A:
B:
C:
Lc:
Rp:
1
2
60
o
7 mm.
60
o
6 mm.
0.2 mm.
T4 T8
D:
F:
A:
B:
C:
Lc:
Rp:
1
3
30
o
7 mm.
100
o
6 mm.
0.4 mm.
D:
F:
A:
B:
C:
Lc:
Rp:
8
5
60
o
7,5 mm.
100
o
6 mm.
0.4 mm.
T9 T10
D:
L:
R:
Lc:
Rp:
1
100 mm.
10 mm.
10 mm.
0 mm.
D:
F:
A:
B:
C:
Lc:
Rp:
1
5
50
o
5 mm.
65
o
5 mm.
0.1 mm.
T11 T12
D:
F:
A:
B:
C:
Lc:
Rp:
1
2
50
o
5 mm.
65
o
5 mm.
0.1 mm.
D:
F:
A:
B:
C:
Lc:
Rp:
1
3
90
o
4 mm.
90
o
4 mm.
0 mm.
T13 T15
D:
F:
A:
B:
C:
Lc:
Rp:
1
6
90
o
4 mm.
90
o
4 mm.
0 mm.
D:
L:
R:
Lc:
Rp:
1
40 mm.
5 mm.
10 mm.
0 mm.
T16 T17
D:
L:
R:
Lc:
Rp:
1
40 mm.
5 mm.
5 mm.
0 mm.
D:
F:
A:
B:
C:
Lc:
Rp:
1
2
40
o
7 mm.
70
o
6 mm.
0.2 mm.
Examples manual (·T· model)
CNC 8070
BASIC CONCEPTS
Part zero setting
1.
(REF: 0706)
5
1.3 Part zero setting
The part zero must be placed so it simplifies the conversion of part dimensions into
program coordinates.
If no part zero is set, the active part zero that all the coordinates are referred to will
be the machine reference zero. Here is a short description of two methods to set the
part zero.
Coordinate preset "G92"
When presetting a coordinate, the CNC interprets that the axis coordinates
programmed after the "G92" set the current position of the axes.
Zero offset "G54" through "G59"/"G159"
In order to apply a zero offset, it must have been previously defined. To do that, the
CNC has a table where the operator may define up to 20 different zero offsets. The
first 6 from "G54" to "G59", the reset from "G159=7" to "G159=20". The table data
may be defined:
• Manually, from the front panel of the CNC.
• By program, assigning the corresponding value (of the "n" offset and of the "Xn"
axis) to the "V.A.ORGT[n].Xn" variable.
Part zero cancellation, "G53"
The part zero stays active until it is canceled with a preset, a zero offset or with a
"G53".
Example: check
G90 G00 X32 Z120 ; Tool approach
G01 X0 ; Facing and positioning in (120,0)
G92 X0 Y0 ; Presetting (120,0) as part zero
Press the key to access the user tables (zero offsets, fixture offsets, etc.)
Access the zero offset table by pressing "F1".
After placing the cursor in the cell to be modified, key in the value and
press [ENTER]
Example:
V.A.ORGT[1].X=0 V.A.ORGT[1].Z=120 ; Assigns the values X=0 Z=120 to the 1st datum
point
G54 ; Applies the first zero offset, same as
programming G159=1.
Examples manual (·T· model)
CNC 8070
1.
BASIC CONCEPTS
Programming of machining conditions.
(REF: 0706)
6
1.4 Programming of machining conditions.
Setting the feedrate in the part-program, "G94/G95"
• "G94",millimeters/minute (inches/minute).
The feedrate is independent from the spindle speed.
• "G95", millimeters/turn (inches/turn).
The feedrate varies with the spindle speed and it will be the typical lathe
configuration.
The default type of feedrate is set in G.M.P. "IFFEED".
Setting the spindle speed in the part-program, "G96/G97"
• "G96", constant surface speed when varying the turning speed (CSS).
A maximum turning speed should be programmed because the smaller the
diameter is the faster the spindle turns. The turning speed limit is programmed
using function "G192". Speed set in rpm, examples.
G192 S1000
G192 S1=500
• "G97", constant turning speed when varying the cutting speed (RPM).
Technical specifications
Type of machine
• CNC lathe.
• Configuration of "plane" type axes (M.P. GEOCONFIG = PLANE).
The work plane is G18 and will be formed by the first two axes defined in the
channel. If the X (first) and Z (second) axes have been defined, the work plane
will be the ZX (Z as abscissa and X as ordinate). There may be more axes, but
they must be auxiliary, rotary, etc.
The cutting speeds and feedrates shown in this manual are for orientation
purposes only and they may be different depending on type of material of the
part and on the tools. When machining one of the parts of these examples,
use the speeds recommended by the manufacturer of the machine. The tool
number will also be different depending on the machine.
Examples manual (·T· model)
CNC 8070
BASIC CONCEPTS
Coordinate programming
1.
(REF: 0706)
7
1.5 Coordinate programming
Absolute coordinates "G90" or incremental coordinates
"G91" .
Absolute: The coordinates of the point are referred to the current (active)
origin of the coordinate system, usually the part zero.
Incremental: The coordinates of the point are referred to the current tool
position.
By default, the machine manufacturer sets it in G.M.P. "ISYSTEM"
Programming in radius "G152"or in diameters "G151".
Programming in diameters is only available on the axes allowed by the machine
manufacturer (DIAMPROG=YES).
Programming in radius. Programming in diameters.
Examples manual (·T· model)
CNC 8070
1.
BASIC CONCEPTS
Coordinate programming
(REF: 0706)
8
1.5.1 Example 1: Absolute and incremental coordinates
Programming in radius
Programming in diameters (only if X axis M.P DIAMPROG = yes)
; Absolute "G90" ; Incremental "G91"
G90 G95 G96 F0.15 S180 T2 D1 M4 M41 G90 G95 G96 F0.15 S180 T2 D1 M4 M41
G0 X50 Z100 G0 X50 Z100
G1 X0 Z80 ; Point A G1 X0 Z80 ; Point A
G1 X15 Z65 ; A-B section G1 G91 X15 Z-15 ; A-B section
Z55 ; B-C section Z-10 ; B-C section
X40 Z30 ; C-D section X25 Z-25 ; C-D section
Z0 ; D-E section Z-30 ; D-E section
G0 X50 Z100 G0 G90 X50 Z100
M30 M30
; Absolute "G90" ; Incremental "G91"
G90 G95 G96 F0.15 S180 T2 D1 M4 M41 G90 G95 G96 F0.15 S180 T2 D1 M4 M41
G0 X100 Z100 G0 X100 Z100
G1 X0 Z80 ; Point A G1 X0 Z80 ; Point A
G1 X30 Z65 ; A-B section G1 G91 X30 Z-15 ; A-B section
Z55 ; B-C section Z-10 ; B-C section
X80 Z30 ; C-D section X50 Z-25 ; C-D section
Z0 ; D-E section Z-30 ; D-E section
G0 X100 Z100 G0 G90 X100 Z100
M30 M30
Examples manual (·T· model)
CNC 8070
BASIC CONCEPTS
Tool path programming
1.
(REF: 0706)
9
1.6 Tool path programming
G00 Rapid traverse.
G01 Linear interpolation.
G02 Clockwise circular interpolation.
G03 Counterclockwise circular interpolation.
Two ways of programming Cartesian coordinates.
G36 Corner rounding, radius blend.
G37 Tangential entry.
G38 Tangential exit.
G39 Corner chamfering.
They must be programmed alone in the block. The programming format is "G3..I"
where "I" is the radius of the chamfer, "I" stays active for all four G functions until it
is changed.
G40 Cancellation of tool radius compensation.
G41 Left-hand tool radius compensation.
G42 Right-hand tool radius compensation.
The tool will position to the left or to the right of the programmed path, according to
the machining direction.
By setting the end point and the
radius
By setting the end point and the
center
G02/G03 X Z R G02/G03 X Z I K
Radius sign
Arc 1: G02 X... Z... R-...
Arc 2: G02 X... Z... R+...
Arc 3: G03 X... Z... R+...
Arc 4: G03 X... Z... R-...
Z
X
R
X,Z
Z
X
I
K
X,Z
Z
X
1
2
3
4
Without compensation. With compensation.
Z
X
Z
X
Examples manual (·T· model)
CNC 8070
1.
BASIC CONCEPTS
Tool path programming
(REF: 0706)
10
1.6.1 Example 2: Arc programming "G02/G03".
Programming in radius
Programming using the arc center
Programming using the arc radius
; Absolute "G90" ; Incremental "G91"
G90 G95 G96 F0.15 S180 T2 D1 M4 G90 G95 G96 F0.15 S180 T2 D1 M4
G0 X60 Z120 G0 X60 Z120
G1 X0 Z90 ; Point A G1 X0 Z90 ; Point A
G3 X20 Z70 I0 K-20 ; A-B section G91 G3 X20 Z-20 I0 K-20 ; A-B section
G1 Z60 ; B-C section G1 Z-10 ; B-C section
G2 X30 Z30 I50 K0 ; C-D section G2 X10 Z-30 I50 K0 ; C-D section
G1 X40 ; D-E section G1 X10 ; D-E section
G3 X50 Z10 I-19.9 K-22.45 ; E-F section G3 X10 Z-20 I-19.9 K-22.45 ; E-F section
G1 Z0 ; F-G section G1 Z-10 ; F-G section
G0 X60 Z120 G0 G90 X60 Z120
M30 M30
; Absolute "G90" ;Incremental "G91"
G90 G95 G96 F0.15 S180 T2 D1 M4 G90 G95 G96 F0.15 S180 T2 D1 M4
G0 X60 Z120 G0 X60 Z120
G1 X0 Z90 ; Point A G1 X0 Z90 ; Point A
G3 X20 Z70 R20 ; A-B section G91 G3 X20 Z-20 R20 ; A-B section
G1 Z60 ; B-C section G1 Z-10 ; B-C section
G2 X30 Z30 R50 ; C-D section G2 X10 Z-30 R50 ; C-D section
G1 X40 ; D-E section G1 X10 ; D-E section
G3 X50 Z10 R30 ; E-F section G3 X10 Z-20 R30 ; E-F section
G1 Z0 ; F-G section G1 Z-10 ; F-G section
G0 X60 Z120 G0 G90 X60 Z120
M30 M30
Examples manual (·T· model)
CNC 8070
BASIC CONCEPTS
Tool path programming
1.
(REF: 0706)
11
Programming in diameters
Programming using the arc center
Programming using the arc radius
;Absolute "G90" ;Incremental "G91"
G90 G95 G96 F0.15 S180 T2 D1 M4 G90 G95 G96 F0.15 S180 T2 D1 M4
G0 X120 Z120 G0 X120 Z120
G1 X0 Z90 ;Point A G1 X0 Z90 ;Point A
G3 X40 Z70 I0 K-20 ;A-B section G91 G3 X40 Z-20 I0 K-20 ;A-B section
G1 Z60 ;B-C section G1 Z-10 ;B-C section
G2 X60 Z30 I50 K0 ;C-D section G2 X20 Z-30 I50 K0 ;C-D section
G1 X80 ;D-E section G1 X20 ;D-E section
G3 X100 Z10 I-19.9 K-22.45 ;E-F section G3 X20 Z-20 I-19.9 K-22.45 ;E-F section
G1 Z0 ;F-G section G1 Z-10 ;F-G section
G0 X120 Z120 G0 G90 X120 Z120
M30 M30
;Absolute "G90" ;Incremental "G91"
G90 G95 G96 F0.15 S180 T2 D1 M4 G90 G95 G96 F0.15 S180 T2 D1 M4
G0 X120 Z120 G0 X120 Z120
G1 X0 Z90 ;Point A G1 X0 Z90 ;Point A
G3 X40 Z70 R20 ;A-B section G91 G3 X40 Z-20 R20 ;A-B section
G1 Z60 ;B-C section G1 Z-10 ;B-C section
G2 X60 Z30 R50 ;C-D section G2 X20 Z-30 R50 ;C-D section
G1 X80 ;D-E section G1 X20 ;D-E section
G3 X100 Z10 R30 ;E-F section G3 X20 Z-20 R30 ;E-F section
G1 Z0 ;F-G section G1 Z-10 ;F-G section
G0 X120 Z120 G0 G90 X120 Z120
M30 M30
Examples manual (·T· model)
CNC 8070
1.
BASIC CONCEPTS
Tool path programming
(REF: 0706)
12
1.6.2 Example 3: Tangential entry/exit "G37/G38" and corner rounding
(radius blend) "G36" with tool radius compensation
"G40/G41/G42".
Programming using the arc center:
;Absolute "G90"
G90 G95 G96 F0.15 S180 T2 D1 M4
G0 X120 Z120
G42 X0 ; Beginning of tool radius compensation.
G01 X0 Z100
G37 I4 ; Tangential entry to point A
G01 X40 ; A-B section
G36 I5 ; Rounding B
G01 Z70 ; B-C section
G36 ; Rounding C (the radius I stays active until it is changed)
G01 X60 Z50 ; C-D section
G36 ; Rounding D
G01 X80 ; D-E section
G36 ; Rounding E
G01 Z30 ; E-F section
G36 ; Rounding F
G01 X100 Z20 ; F-G section
G36 ; Rounding G
G01 Z0 ; G-H section
G38 I4 ; Tangential exit.
G0 X120
G40 Z120 ; End of tool radius compensation.
M30
13
CNC 8070
(REF: 0706)
2
CANNED CYCLE
PROGRAMMING
2.1 Introduction
The canned cycles edited in ISO code are defined using a "G" function and its relevant
parameters.
• G81 Turning cycle with straight sections.
• G82 Facing cycle with straight sections.
• G83 Drilling / tapping canned cycle.
• G84 Turning cycle with circular sections.
• G85 Facing cycle with circular sections.
• G86 Longitudinal threading.
• G87 Face threading.
• G88 Grooving cycle along X axis.
• G89 Grooving cycle along Z axis.
• G66 Pattern repeat cycle.
• G68 Stock removal along the X axis.
• G69 Stock removal along the Z axis.
Machining canned cycles with a live tool:
• G160 Drilling / tapping canned cycle on the face of the part.
• G161 Drilling / tapping canned cycle on the side of the part.
• G162 Slot milling canned cycle along the side of the part.
• G163 Slot milling canned cycle along the face of the part.
A canned cycle may be defined anywhere in the program, that is, in the main program
as well as in a subroutine.
Examples manual (·T· model)
CNC 8070
2.
CANNED CYCLE PROGRAMMING
Example 4. Inside turning of curved and straight sections.
(REF: 0706)
14
2.2 Example 4. Inside turning of curved and straight
sections.
Dim. rough stock Ø80x114mm
;First fixture
;Set the part zero.
V.A.ORGT[1].X=0 V.A.ORGT[1].Z=112
G54
G192 S2200
;Operation 1 (Drilling)
G94 G97 F90 S600 M4
Z150 (default feedrate according to M.P. IMOVE = G0/G1)
T9 D1
G0 X0 Z8
G83 X0 Z0 I45.773 B9 D4 K0 H0 C1
;Operation 2 (Inside curved turning)
G95 G96 F0.2 S120 M4
T8 D8
G0 X20 Z20
G1 G41 X18 Z5
G84 X70 Z0 Q20 R-33.541 C2 L0.3 M0.3 H0.1 I-35 K0
G0 G40 Z150
;Operation 3 (Outside facing and turning)
G95 G96 F0.2 S180 M4
T2 D1
G0 X90 Z20
G1 X78 Z5
G1 Z-40
G1 X85
G0 Z0
G1 X66
G1 Z5
G1 G42 X72 Z1
G1 X80 Z-3
G0 G40 Z150
Z
X
1
Z
X
2
Z
X
3
Page is loading ...
Page is loading ...
Page is loading ...
Page is loading ...
Page is loading ...
Page is loading ...
Page is loading ...
Page is loading ...
Page is loading ...
Page is loading ...
Page is loading ...
Page is loading ...
Page is loading ...
Page is loading ...
Page is loading ...
Page is loading ...
Page is loading ...
Page is loading ...
Page is loading ...
Page is loading ...
Page is loading ...
Page is loading ...
Page is loading ...
Page is loading ...
Page is loading ...
Page is loading ...
Page is loading ...
Page is loading ...
Page is loading ...
Page is loading ...
Page is loading ...
Page is loading ...
Page is loading ...
Page is loading ...
Page is loading ...
Page is loading ...
Page is loading ...
Page is loading ...
/
