Siemens SINUMERIK 802D Installation guide

SINUMERIK 802D solution line
Machine Controller Milling Handbook
Training Manual Edition 2006.7
Training Material

SINUMERIK 802D sl
Operating, Programming
and Service
Milling
Valid for
Control Software
SINUMERIK 802D sl 1.2
Edition 07.2006

Module content for end users.
Operating and Programming
CNC Basic Principles Milling C102
Basic Program Structure C98
Modality (preparatory functions) C89
Commonly used G functions - M C92
Basic Miscellaneous Codes C97
Additional G functions - M C94
Create part program - Milling C77
Cycles - M C99
File Management - CF card C59
Power On and Referencing C69
Axis Control - Jog C82
Control Structure / Navigation C70
MDA - Milling C76
Tools Turning—Milling functions C83
Tools Milling - work planes C72
Work offsets - Milling C74
Automatic C81
RCS 802 Data transfer tool C1
ISO Dialect programming - M C95
Service
Pushbutton test (MCP) C8
LED Diagnosis Drive C9
LED Diagnosis HMI C10
MCPA signal test C11
Save Data Backup C17
Restore Data Backup C18
External data backup and restore C19
Diagnose PLC program C28
Diagnose PLC alarm C31
PLC periphery (HW diagnosis) C32
Alarm structure C37
Editing of NC Machine data C41
Drive Diagnostic parameters C53

SINUMERIK 802D sl Operating and Service Training Manual Page 1 C102 C102
CNC Basic Principles Milling
C102
1 Brief description
Module Objective:
Upon completion of this module you can understand the basic functionality and requirements of a
CNC controller
Module description:
CNC machines replicate the functions of a manual machine through the use of a sequential program,
this program replicates the movements of a manual machine through the so called “CNC program” .
Geometric relationships of the component to the machine are achieved with (Tool and component)
numeric compensations. These compensations mathematically compensate the difference between
component, Tool and machine.
• Fundamentals of CNC Machines
Module Content:
Fundamentals of CNC
Machines Section 2

Notes
SINUMERIK 802D sl Operating and Service Training Manual Page 2 C102 C102
Fundamentals of CNC Machines
Section 2
The difference between a Manual machine and a CNC machine is a logical
difference based upon numerical values. This overview module and the
following CNC modules should help explain the myth of CNC.
ITS ONLY NUMBERS. No magic !!
Reference position Z
Reference position X
Zero Offset
Tool Offset
Zero Offset

SINUMERIK 802D sl Operating and Service Training Manual Page 1 C98 C98
Basic program structure
C98
1 Brief description
• Basic structure
• Basic structure for turning
• Basic structure for milling
Basic structure for
turning
Basic structure for
milling
Section 3
Section 4
Basic structure
Section 2
Module objective:
Upon completion of this module you will understand the basic structure of an NC program
Module description:
We use a basic structure when writing a program to give some kind of order to the program, this will
also help when performing a “Block search”.
Module content:

Notes
SINUMERIK 802D sl Operating and Service Training Manual Page 2 C98 C98
Section 2 Basic structure
2.1 Basic structure of NC program
There are five basic parts to an NC program.
1. Basic startup G functions.
2. Call tool and set spindle speed, feed, coolant.
3. Set geometry to cut component.
4. Tool to safe position
5. End of program
G00 G90 G94 G40 G17 G71 Basic G functions for program
T1
M
6 Call tool etc
G95 S1500 F0.15 M08
G00 G54 X0.0 Y0.0 Z50.0
….
….
….
…
. Geometry for component
….
….
….
G00 G40 Z50.0
X0.0 Y200.0 Z200.0 Safe position for tool change
M30 End of program
You will note that for each tool there is always :
• Call tool etc
• Geometry for component
• Safe position for tool change
This will be the same for ever tool that is written in the NC program
If you keep to a good basic structure, this will make the program safer to
run and easier to perform a block search.

Notes
SINUMERIK 802D sl Operating and Service Training Manual Page 3 C98 C98
Section 3 Basic structure for turning
3.1 Basic structure of NC program for turning
N10 G00 G90 G95 G40 G18 G71
N20
LIMS=2500 Basic G functions for program
N30 G54
N40 T1 D1
N50
G18 Call tool etc
N60 G96 S250 M03 M08
N70 G00 X52.0 Z0.1
N80 G01 X-2.0 F0.15
N90 G00 Z2.0
N100 X20.0
N110 G01 Z-20.0 Geometry for component
N120 X30.0 Z-25.0
N130 X45.0
N140 Z-50.0
N150 X52.0
N160 G00 G40 Z2.0
N170 X200.0 X1200.0 Safe position for tool change
N180 T4 D1
N190
G17 Call tool etc
N200 G95 S1500 M04 M08
N210 G00 X0.0 Z2.0
N220 G01 Z-25.0 F0.25 Geometry for component
N230 G00 Z2.0
N240 G00 G40 Z2.0
N250 X0.0 Z200.0 Safe position for tool change
N260 M30
End of program

Notes
SINUMERIK 802D sl Operating and Service Training Manual Page 4 C98 C98
Section 4 Basic structure for milling
4.1 Basic structure of NC program for milling
N10 G00 G90 G94 G40 G17 G71 Basic G functions for program
N20 T1
N30
M6 Call tool etc
N40 G95 S2500 F0.25 M03 M08
N50 G00 G54 X0.0 Y0.0 Z50.0
N60 MCALL CYCLE82(5.0. 0.0, 2.0, -2.0, 0.0, 0.0)
N70 X10.0
N80 X20.0
N90
X20.0 Geometry for component
N100 X30.0
N110 X40.0
N120 X50.0
N130 MCALL
N140 G00 G40 Z50.0
N150 X0.0 Y200.0 Z200.0 Safe position for tool change
N160 T4
N170
M06 Call tool etc
N180 G95 S1500 F0.25 M05 M08
N190 G00 G54 X0.0 Y0.0 Z50.0
N200 MCALL CYCLE82(5.0. 0.0, 2.0, -10.0, 0.0, 0.0)
N210 X10.0
N220 X20.0
N230
X20.0 Geometry for component
N240 X30.0
N250 X40.0
N260 X50.0
N270 MCALL
N280 G00 G40 Z50.0
N290 X0.0 Y200.0 Z200.0 Safe position for tool change
N300 M30
End of program

SINUMERIK 802D sl Operating and Service Training Manual Page 1 C89 C89
Modality (Preparatory functions)
C89
1 Brief description
Module objective:
Upon completion of this module you will understand Preparatory functions (G-Codes).
Module description:
We use preparatory G functions according to there appropriate functional group to instruct a machine
what to do via the customers NC program.
Module content:
• G function overview
• G function window display
G function window dis-
play Section 3
G function overview
Section 2

Notes
SINUMERIK 802D sl Operating and Service Training Manual Page 2 C89 C89
Section 2 G function overview
2.1 G function overview
G function (preparatory function).
The G functions are divided into G groups.
Only one G function from each group can be written in a single block.
A G function can either be modal (until canceled by another function from
the same group), or non-modal (only effective for that block it is written
in).
Modal example:
G00 G90 G94 G40 G17
T1 D1
G54 S1000 M03
G01 X0.0 Y0.0 Z0.0 F200
X100.0
Y100.0
X0.0
Y0.0
G00 Z50.0
M30
These blocks are per-
formed at a given feed
rate, because G01 is
modal and will not
change until another
code from the same
group is entered
At this block the speed
of motion will change
due to the change of the
G function group, from
G01 to G00.
Non-modal example:
G00 G90 G94 G40 G17
T2 D1
G54 S1000 M03
X0.0 Y0.0 Z50.0
G01 Z0.0 F200
G04 F10.0
G00 Z50.0
M30
This G function is only
effective in this block, to
use this function again
you must type it in again
in another block.

Notes
SINUMERIK 802D sl Operating and Service Training Manual Page 3 C89 C89
Section 2 G function overview
Group 1: Modally valid motion commands
Name Meaning Machine
G00 Rapid
traverse M/T
G01*# Linear interpolation M/T
G02 Circular interpolation clockwise M/T
G03 Circular interpolation counter-clockwise M/T
G33 Thread cutting with constant lead M/T
Group 2: Non-modally valid motion, dwell
Name Meaning Machine
G04 Dwell time preset M/T
G63 Tapping without synchronization M/T
G74 Reference point approach with synchronization M/T
G75 Fixed point approach M/T
Group 3: Programmable frame, working area limitation
Name Meaning Machine
TRANS Translation,
programmable M/T
ROT Rotation, programmable M/T
SCALE Scaling, programmable M/T
MIRROR Mirroring, programmable M/T
G26 Maximum working area limitation/spindle speed limi-
tation M/T
G25 Minimum working area limitation/spindle speed limita-
tion M/T
Group 6: Plane selection
Name Meaning Machine
G17# Plane selection 1st - 2nd geometry axis M/T
G18* Plane selection 3rd - 1st geometry axis M/T
G19 Plane selection 2nd - 3rd geometry axis M/T
Default for turning * / default for milling #
M = milling / T = turning

Notes
SINUMERIK 802D sl Operating and Service Training Manual Page 4 C89 C89
Section 2 G function overview
Group 11: Exact stop, non-modal
Name Meaning Machine
G09 Velocity reduction, exact positioning M/T
Group 10: Exact stop - continuous-path mode
Name Meaning Machine
G60*# Velocity reduction, exact positioning M/T
G64 Continuous – path mode M/T
Group 9: Frame suppression
Name Meaning Machine
G53 Suppression of current zero offset: including active
settable frame G54 - G59 M/T
Group 8: Settable zero offset
Name Meaning Machine
G500*# Deactivate all settable G54—G59 if G500 not contain
a value M/T
G54 Settable zero offset M/T
G55 Settable zero offset M/T
G56 Settable zero offset M/T
G57 Settable zero offset M/T
G58 Settable zero offset M/T
G59 Settable zero offset M/T
Group 7: Tool radius compensation
Name Meaning machine
G40*# No tool radius compensation M/T
G41 Tool radius compensation left of contour M/T
G42 Tool radius compensation right of contour M/T
Default for turning * / default for milling #
M = milling / T = turning

Notes
SINUMERIK 802D sl Operating and Service Training Manual Page 5 C89 C89
Section 2 G function overview
Group 16: Feed override on inside and outside curvature
Name Meaning Machine
CFC*# Constant feed at contour M/T
CFTCP Constant feed in tool center point (center-point path) M/T
CFIN Constant feed at internal radius, acceleration at exter-
nal radius M/T
Group 15: Feed type
Name Meaning Machine
G94# Linear feed mm/min, inch/min M/T
G95* Rotational feed in mm/rev, inch/rev M/T
G96 Constant cutting speed (type of feed as for G95) ON T
G97 Constant cutting speed (type of feed as for G95) OFF T
Group 14: Workpiece measuring absolute/incremental
Name Meaning Machine
G90*# Absolute dimensions input M/T
G91 Incremental dimension input M/T
Group 13: Workpiece measuring inch/metric
Name Meaning Machine
G70 Input system inches (lengths) M/T
G71*# Input system metric (lengths) M/T
Default for turning * / default for milling #
M = milling / T = turning

Notes
SINUMERIK 802D sl Operating and Service Training Manual Page 6 C89 C89
Section 3 G function window display
3.1 G function window display
To look at the active G-codes, you can activate a window called
G FUNCTION.
PRESS
PRESS
This “G function” softkey is present in modes:
Softkey G function

Notes
SINUMERIK 802D sl Operating and Service Training Manual Page 7 C89 C89
Section 3 G function window display
This is what you will see:
This is the window
that is shown.
In this window, it will show you every group number and the active G-code
for that group at that present time.
Use the button
to scroll down or up to search for the required G-code group.
This shows you the
group number.
Page
up Page Down
This is the window
that is shown.
The slide bar has
now moved.

SINUMERIK 802D sl Operating and Service Training Manual Page 8 C89 C89