SINUMERIK 802D
Brief Instructions 11.2000 Edition
Milling
User Documentation
SINUMERIK 802D
Milling
Valid for
Control Software version
SINUMERIK 802D 1
11.2000 Edition
SINUMERIK® documentation
Printing history
Brief details of this edition and previous editions are listed
below.
The status of each edition is shown by the code in the
"Remarks" column.
Status code in the "Remarks" column:
A .... New documentation.
B .... Unrevised reprint with new Order No.
C .... Revised edition with new status.
Edition Order No. Remark
11.00 6FC5298-1AA40-0BP0 A
This manual is included in the documentation on CD-ROM
(DOCONCD)
Edition Order No. Remark
08.01 6FC5298-6CA00-0BG1 C
Trademarks
SIMATIC®, SIMATIC HMI®, SIMATIC NET®, SIROTEC®,
SINUMERIK® and SIMODRIVE® are registered trademarks of
Siemens AG. Other names in this publication might be
trademarks, whose use by a third party for his own purposes
may violate the rights of the registered holder.
Further information is available on the Internet under:
http://www.ad.siemens.de/sinumerik
This publication was produced with WinWord V 7.0 and
Designer V 8.0
Other functions not described in this documentation might be executable in the control.
This does not, however, represent an obligation to supply such functions with a new
control or when servicing.
Subject to technical change without prior notice.
The reproduction, transmission or use of this document or its contents is not permitted
without express written authority. Offenders will be liable for damages. All rights,
including rights created by patent grant or registration of a utility model or design are
reserved.
© Siemens AG 2000. All Rights Reserved.
General Information 11.00
Introduction
How to use this booklet
This manual is a brief instruction manual which describes
all of the
important operator control and programming steps.
Detailed description of the operator control and
programming for Sinumerik 802D:
" User Manual, Turning,
Order No. 6FC5698-2AA00-0BP0
" User Manual, Milling
Order No. 6FC5698-2AA10-0BP0
Description schematic
This description is structured as follows:
Operator control
Prerequisites
Operating sequence
Programming
Programming of the function
Meaning of the parameters
Explanatory illustration with an example of a
workpiece
© Siemens AG 2000. All rights reserved.
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition. 0-5
List of sections 11.00
List of sections
1. Setting-Up 1-9
Tool offsets and compensation.......................................1-10
Measure tool ...................................................................1-11
Determine workpiece zero ..............................................1-12
Enter the zero offset........................................................1-13
2. Generate/Edit Program 2-15
Set-up/open program......................................................2-16
Insert/edit block...............................................................2-17
Copy/insert/delete block .................................................2-18
Search/number the block................................................2-19
Start/simulate program ...................................................2-20
3. Commission/Correct Program 3-23
Select program ...............................................................3-24
Correct program..............................................................3-25
Block search ...................................................................3-26
Trace machining on the screen ......................................3-27
4. Program Path Data 4-29
Absolute and incremental dimensions, G90, G91 ..........4-30
Zero offset, G54 to G59 ..................................................4-31
Selection of working plane G17 to G19 ..........................4-32
5. Programming Axis Motion 5-33
Rapid traverse, G0..........................................................5-34
Linear interpolation, G1 ..................................................5-35
Circular interpolation, G2/G3 ..........................................5-36
Circular interpolation through intermediate point, CIP ....5-38
Rigid tapping, G331/G332 ..............................................5-39
Tapping with floating tap holder, G63 .............................5-40
Polar coordinates G110, G111, G112.............................5-41
6. Tool Offsets and Compensation 6-43
Tool call ..........................................................................6-44
Cutter radius path compensation, G41/G42 ...................6-45
Tool nose radius compensation, G41/G42 .....................6-46
Approach/exit contour, NORM/KONT .............................6-47
Move along the contour, G450/G451..............................6-48
© Siemens AG 2000. All rights reserved.
0-6 SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
11.00 List of sections
List of sections
7. Coordinate Systems 7-49
Frame concept................................................................7-50
Shift/rotate coordinates, TRANS/ROT ............................7-51
Mirroring the coordinate axes, MIRROR .........................7-52
Increasing/reducing size of contour, SCALE ..................7-53
8. Programming Preparatory Functions 8-55
Exact stop, G9/G60.........................................................8-56
Feed in continuous path mode, G64...............................8-57
Programming the spindle motion ....................................8-58
Subroutine technique......................................................8-59
9. Attachment 9-61
List of M commands........................................................9-62
List of G functions ...........................................................9-63
Notes ..............................................................................9-68
© Siemens AG 2000. All rights reserved.
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition. 0-7
e& Siemens AG 2000. All rights reserved.
0-8 SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
1. Setting-Up
Tool offsets and compensation 1-10
Measure tool 1-11
Determine workpiece zero 1-12
Enter the zero offset 1-13
© Siemens AG 2000. All rights reserved. 1-9
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
1. Setting-Up 11.00
Tool offsets and compensation
Prerequisite:
JOG mode selected
Selection
Select
OFFSET
PARAM OFFSET PARAM operating
area
Select "Tool list" menu
Tool
list
Functions
Determine the tool offset data
Measure
tool
Delete the tool offsets
Delete
tool
Display all of the tool
Expanded
parameters
Set-up additional cuts
Cut
Search for tool
Search
Set-up new tool.
New
Enter the new values.
tool
1-10 © Siemens AG 2000. All rights reserved.
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
11.00 1. Setting-Up
Measure tool
Prerequisite:
The tool must be changed-over using the MDA mode.
Then select the JOG mode.
[M] If required, select the
POSITION
[M] POSITION operating area
Select "Measure tool" menu,
Measure
possibly enter the tool number
tool
in the "T" field
Select the required axis in the
"measure tool" window using
the cursor, and enter the
position of the tool tip.
Select length or diameter
Length Diameter
offset (toggle key)
The length and diameter value
Set Set
which are being
length diameter
The diameter of the tool tip is
determined and saved.
© Siemens AG 2000. All rights reserved. 1-11
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
1. Setting-Up 11.00
Determine workpiece zero
Prerequisite:
The tool must be changed-over using the MDA mode.
Then select the JOG mode.
[M] If required, select the
POSITION
[M] POSITION operating area
Select the menu
Measure
"measurement workpiece"
workpiece
Approach workpiece
Select reference axis
X
Y
Z
Enter a possible offset in the
"set position to" field
The system accepts the
Set
calculated result, and this is
zero offset
displayed in the "Zero offset"
field.
1-12 © Siemens AG 2000. All rights reserved.
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
11.00 1. Setting-Up
Enter the zero offset
Select the
OFFSET
PARAM
OFFSET PARAM operating
area
Select the "Zero offset" menu.
Zero
offset
Select the zero offset using
the cursor:
" Basis
" Selectable (G54 to G59)
Enter/change value.
© Siemens AG 2000. All rights reserved. 1-13
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
1. Setting-Up 11.00
1-14 © Siemens AG 2000. All rights reserved.
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
2. Generate/Edit Program
Set-up/open program 2-16
Insert/edit block 2-17
Copy/insert/delete block 2-18
Search/number the block 2-19
Start/simulate program 2-20
© Siemens AG 2000. All rights reserved. 2-15
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
2. Generate/Edit Program 11.00
Set-up/open program
Set-up new program:
PROGRAM
Select the
MANAGER
PROGRAM MANAGER
operating area
Select program directory
Programs
Enter program name and
New
acknowledge with OK
OK
Please note:
For subroutines, the "SPF" file ID must be explicitly written-
out (e.g. TEST.SPF).
Open the existing program:
PROGRAM
Select the
MANAGER
PROGRAM MANAGER
operating area
Select program directory
Programs
Select the program using the
cursor in the program directory
and
open.
Open
Note:
If the program was already previously opened in the editor,
it can be directly selected using the PROGRAM operating
area key.
2-16 © Siemens AG 2000. All rights reserved.
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
11.00 2. Generate/Edit Program
Insert/edit block
Insert new block
Prerequisite:
The existing program has been opened.
Select the insert line using the
cursor
Press the input key
Edit block
Prerequisite:
The existing program has been opened.
Select and change the block
using the cursor.
Note:
If the program was already previously opened in the editor,
it can be directly selected using the PROGRAM operating
area key.
© Siemens AG 2000. All rights reserved. 2-17
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
2. Generate/Edit Program 11.00
Copy/insert/delete block
Copy/insert
Prerequisite:
The existing program has been opened.
Using the cursor, select the
required block or position,
which should be marked from
there onwards,
Start marking
Mark
block
Select the end of the marked
range using the cursor
Copy the marked text
Copy
block
Set the write mark at the
required insertion point
Insert the copied marked text
Insert
block
Note:
" The marked text is always inserted after the cursor.
" Blocks can also be copied and inserted between the
various programs.
Delete
Prerequisite:
The existing program has been opened.
Using the cursor, select the
required block or position
which should be marked from
there onwards.
Start marking
Mark
block
Select the end of the marked
range using the cursor
Delete the marked text
Delete
block
2-18 © Siemens AG 2000. All rights reserved.
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
11.00 2. Generate/Edit Program
Search/number the block
Search block
Prerequisite:
The existing program has been opened.
Enter the search text. You can
Search
select between either
Text or line number (for block
Text Line
number, "N..." should be
No.
entered)
Start search
OK
Note:
At the start of text search, you can either
" search from the cursor position or
" search from the start of a block.
Number block
Prerequisite:
The program has been opened.
The block numbers of the
Number
complete program are re-
numbered in steps of 10.
© Siemens AG 2000. All rights reserved. 2-19
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
2. Generate/Edit Program 11.00
Start/simulate program
Start program
Prerequisite:
The automatic mode is selected.
The existing program has been opened.
Select the program which is to
Process
be processed
The program is started using
NC start
2-20 © Siemens AG 2000. All rights reserved.
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
11.00 2. Generate/Edit Program
Simulate program
Prerequisite:
The automatic mode has been selected
The existing program has been opened.
Select simulation and start
Simulation
with NC start
Sub-menu call to display:
Display
...
Select level
Display G17/
(sub-menu to "display...")
G18/G19
Display complete workpiece
Display
(sub-menu to "Display...")
all
Zoom-in at the display section
Zoom +
Zoom-out at the display
Zoom -
section
Select the start display for the
To
simulation
origin
Automatic scaling of the
Zoom
traced tool path
Auto
Change the cursor increment
Cursor
coarse/fine
Delete the simulation display
Delete
display
Return to the edit mode
Edit
© Siemens AG 2000. All rights reserved. 2-21
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
2. Generate/Edit Program 11.00
2-22 © Siemens AG 2000. All rights reserved.
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
3. Commission/Correct Program
Select program 3-24
Correct program 3-25
Block search 3-26
Trace machining on the screen 3-27
© Siemens AG 2000. All rights reserved. 3-23
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
3. Commission/Correct Program 11.00
Select program
PROGRAM
Select the
MANAGER
PROGRAM MANAGER
operating area
Select program directory.
Programs
Select the program using the
cursor in the program directory
and
Select the program which is to
Process
be processed
Select the automatic mode
Start the program with NC
Start
Note:
The following conditions, among others, must be fulfilled to
start the program:
" There may be no alarms.
" The feed is enabled.
" The spindle is enabled.
3-24 © Siemens AG 2000. All rights reserved.
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
11.00 3. Commission/Correct Program
Correct program
NC Stop
Prerequisite:
The program is executed in the automatic mode.
Stop program
Select program correction
Program
correction
Select and correct block using
the cursor.
With NC start, the program is
continued at the point where it
was interrupted.
Note:
" After the program has been interrupted (NC Stop), the
tool can be moved away from the contour in the
manual mode (jog). The control saves the coordinates
at the point of interruption.
" Corrections are only possible in the blocks which have
still not been read-in by the control.
NC reset
Prerequisite:
The program is executed in the automatic mode.
Interrupt program.
Select program correction
Program
correction
Select and correct block using
the cursor.
With the NC Start, the
program is started from the
beginning.
Note:
" When system errors occur in the part program, the
control stops further processing.
© Siemens AG 2000. All rights reserved. 3-25
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
3. Commission/Correct Program 11.00
Block search
Prerequisite:
The program has been selected in the automatic mode and
is being executed.
Interrupt program
Select block search
Block
search
If required, select the higher or
Program Program
lower program level.
level + level -
Select the block in the editor
using the cursor or
Enter the search text and start
Search
the search
OK
Enter changes
You have 4 ways of re-
starting:
" at the beginning of the
To
contour
contour
" at the end of the contour
To
end point
" Without calculating-in the
No
tool offsets
calculation
" at the interruption position
Interrupt
Continue the program with NC
Start
Notice:
A tool change is only taken into account if the tool is
entered in the target block.
3-26 © Siemens AG 2000. All rights reserved.
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
11.00 3. Commission/Correct Program
Trace machining on the screen
Prerequisite:
The program has been selected in the automatic mode.
[M] If required, select the
POSITION
[M] POSITION operating area
Start trace
Trace
Start the program with NC
Start
Workpiece machining is
simultaneously displayed on
the screen
As for the simulation, functions
are also available here for
different display settings
(zoom, to origin, ...)
© Siemens AG 2000. All rights reserved. 3-27
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
3. Commission/Correct Program 11.00
3-28 © Siemens AG 2000. All rights reserved.
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
4. Program Path Data
Absolute and incremental dimensions, G90, G91 4-30
Zero offset, G54 to G59 4-31
Selection of working plane G17 to G19 4-32
© Siemens AG 2000. All rights reserved. 4-29
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
4. Program Path Data 11.00
Absolute and incremental dimensions, G90, G91
N 5 G0 X25 Y15 Z2
G90
N20 G1 X80 F300
G91
Parameters
G90 Absolute dimension input, all data refers to the
actual workpiece zero.
G91 Incremental dimension input, each dimension
refers to the contour point last input.
You can change over from block to block as often as you
want between absolute and incremental data input.
Within a block, you can also change the type of input for
individual axes by specifying AC for absolute coordinates or
IC for incremental coordinates.
Example: X = AC (400)
N5 G00 G90 X25 Y15 Z2
Y
N10 G01 Z-5 F300
X80
N20 G01 G91
+80
N20
25 80
X
Change between absolute and incremental dimension programming
4-30 © Siemens AG 2000. All rights reserved.
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
80
15
5
N
11.00 4. Program Path Data
Zero offset, G54 to G59
N30 ...
N40 G54
N50 G0 X30 Y75
Other zero offsets: G55...G59
X,Y,Z Coordinates of the zero offset (definition of the
workpiece coordinate system) These must
have been entered into the control via the
operating panel or serial interface before
programming.
With command G53, zero offsets can be suppressed block
by block; de-activate with G500.
G54
G55
G56
G57
Zero offsets make multiple machining operations possible
© Siemens AG 2000. All rights reserved. 4-31
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
4. Program Path Data 11.00
Selection of working plane G17 to G19
N10 G0 X50 Z50 G17 D1 F1000
Command Working plane Infeed axis
G17 X/Y Z
G18 Z/X Y
G19 Y/Z X
Programming of the working plane is needed for
computation of the tool offset data.
It is not possible to change the working plane when
G41/G42 is active.
Standard setting: G17
ZZ
G17 G18
Y
Y
X X
Z G19
Y
X
Selection of working planes for horizontal and vertical milling operations
4-32 © Siemens AG 2000. All rights reserved.
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
5. Programming Axis Motion
Rapid traverse, G0 5-34
Linear interpolation, G1 5-35
Circular interpolation, G2/G3 5-36
Circular interpolation
through intermediate point, CIP 5-38
Rigid tapping, G331/G332 5-39
Tapping with floating tap holder, G63 5-40
Polar coordinates G110, G111, G112 5-41
© Siemens AG 2000. All rights reserved. 5-33
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
5. Programming Axis Motion 11.00
Rapid traverse, G0
N10 X0 Y0 Z3
G0
X, Y, Z Coordinates of the target point
Z
Y
N10
X
Fast tool positioning in rapid traverse for milling
5-34 © Siemens AG 2000. All rights reserved.
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
11.00 5. Programming Axis Motion
Linear interpolation, G1
N10 G0 G90 X10 Y10 Z1 S800 M3
N20 G1 Z-12 F500
N30 X30 Y35 Z-3 F700
X, Y, Z Coordinates of the target point
F Feed rate
Z
Y
X
Making a slot
© Siemens AG 2000. All rights reserved. 5-35
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
5. Programming Axis Motion 11.00
Circular interpolation, G2/G3
Center point programming
N5 G0 G90 X35 Y60
N10 G3 X50 Y45 I0 J-15 F500
X, Y, Z Coordinates of the circle end point
I, J, K Interpolation parameters (directions: I in X,
J in Y, K in Z) for determining the circle center
point
With G2 the tool travels clockwise, with G3 counter-
clockwise. Viewing direction along the third coordinate axis.
G3 X50 Y45 I0 J-15 F500
Z
Y
Y
X
Making a circular slot
5-36 © Siemens AG 2000. All rights reserved.
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
0
6
5
4
I
=
0
J
=
-
1
5
3
5
5
0
11.00 5. Programming Axis Motion
Circular interpolation, G2/G3
Radius program
N20 G90 G0 X68 Z102
N30 G90 G3 X20 Z150 CR=48 F300
CR Circle radius
CR=+ Traversed angle > 180°
CR=- Traversed angle > 180°
X, Z, Definition of end point
Radius programming is not allowed if the traversed angle is
360°.
N30 G90 G3 X20 Z150 CR=48
X
Z
102
150
Radius programming from drawing
© Siemens AG 2000. All rights reserved. 5-37
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
Ø 68
Ø 20
8
4
R
5. Programming Axis Motion 11.00
Circular interpolation through
intermediate point, CIP
N10 CIP X87 Y20 I1=60 J1=35
X, Y, Z Coordinates of the circle end point
I1=, J1=, Interpolation parameters for determining the
K1= intermediate point
If the circle parameter point is not given in the production
drawing, you can program circular interpolations with CIP
without additional calculations.
You can also use this function to program circles in space.
Y
I1=60 J1=35
Start
60
35
X
20
50
60
87
Circular interpolation through point
5-38 © Siemens AG 2000. All rights reserved.
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
11.00 5. Programming Axis Motion
Rigid tapping, G331/G332
N40 SPOS=0
N50 G331 Z-50 K2 S500
N60 G332 Z5 K2
SPOS=0 Change spindle to position control and put into
position
G331 Tapping
G332 Tapping with retraction. The spindle changes
direction of rotation automatically
X, Y, Z Thread end point
I, J, K Thread lead. Positive lead (e.g. K4) right-hand
thread, negative lead (e.g. K-4) left-hand
thread.
For this function, the spindle must be equipped with a pulse
encoder.
Z
X
Tapping without floating tap holder (analog to the next page)
© Siemens AG 2000. All rights reserved. 5-39
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
- 50
5. Programming Axis Motion 11.00
Tapping with floating tap holder, G63
N10 G63 Z-50 M3 S...F...
N20 G63 Z4 M4 F...
G63 For the retraction movement, you program
another block with G63 and the relevant
direction of spindle rotation.
S Spindle speed
F Feed rate
M3 Direction of rotation right
M4 Direction of rotation left
Calculation of feed rate:
F = Spindle speed x Thread lead
For this function, you need a thread tap in the floating tap
holder. A spindle pulse encoder is not required.
Z
X
Thread tapping with floating tap holder (analog to the previous page)
5-40 © Siemens AG 2000. All rights reserved.
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
- 50
11.00 5. Programming Axis Motion
Polar coordinates G110, G111, G112
N30 G111 X40 Y35 Z40
N40 G3 RP=... AP=...
G110 Definition of pole, referred to tool position last
programmed
G111 Definition of absolute pole in the workpiece
coordinate system
G112 Definition of pole, referred to pole last valid
X, Y, Z Coordinates of the pole
RP= Radius, distance between pole and target point
AP= Angle between path between pole and target
point and the angle reference axis (pole axis
first named)
The pole (center point) can be defined in rectangular or
polar coordinates.
When programming the circle, the pole is in the circle
center point and RP corresponds to the circle radius.
Z
Z*
Y*
AP
AP
AP
RP
X*
AP
AP
X
Description of travel paths using polar coordinates
© Siemens AG 2000. All rights reserved. 5-41
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
0
3
N
=
5. Programming Axis Motion 11.00
5-42 © Siemens AG 2000. All rights reserved.
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
6. Tool Offsets and Compensation
Tool call 6-44
Cutter radius path compensation, G41/G42 6-45
Tool nose radius compensation, G41/G42 6-46
Approach/exit contour, NORM/KONT 6-47
Move along the contour, G450/G451 6-48
© Siemens AG 2000. All rights reserved. 6-43
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
6. Tool Offsets and Compensation 11.00
Tool call
N10 T17 D8
T Call tool number
D Call tool offset, activate tool length
compensation
In order that the tool offsets are correctly taken into account
in the axes, before the tool is called, the machining plane
must be selected.
Tool offset values can be exchanged in the course of the
NC run. The machining plane does not have to be re-
programmed.
If no D number is to be input when the tool is called, a
D number can be specified via machine data.
N10 T17 D8
...
N30 D6
X
Z
Offset values for left-hand and right-hand tool nose for recessing tool
6-44 © Siemens AG 2000. All rights reserved.
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
11.00 6. Tool Offsets and Compensation
Cutter radius path compensation,
G41/G42
N10 G1 G17 G41 D8 X... Y... Z... F500
G41 Call for path correction; tool motion in the
traversing direction left of the contour
G42 Call for path correction, tool motion in the
traversing direction right of the contour
G40 Deselection of cutter path compensation
The tool length compensation acts automatically after tool
offset D has been called.
In the NC block with G40/G41/G42, there must be at least
one axis programmed with the selected working plane (G17
to G19).
The CRC must be selected and de-selected in a
program block with G0 or G1.
The offset acts only in the programmed working plane
(G17 to G19).
Z
Y
G42
G41
X
Milling radius - path correction left or right of the programmed path
© Siemens AG 2000. All rights reserved. 6-45
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
6. Tool Offsets and Compensation 11.00
Tool nose radius compensation, G41/G42
N5 G90 G0 G41 D... X... Y... Z...
G41 Call for radius compensation, tool motion in
traversing direction left of workpiece
G42 Call for radius compensation, tool motion in
traversing direction right of workpiece
G40 Deselection of radius compensation
In the NC block with G40/G41/G42, there must be at least
one axis programmed with the selected working plane (G17
to G19).
The compensation must be selected and deselected in a
program block with G0 or G1. The compensation acts only
in the programmed working plane (G17 to G19).
a= without cutting radius compensation
b= with cutting radius compensation
G42
a
G41
...D...
b
Tool nose radius compensation for machining slopes and circular arcs
6-46 © Siemens AG 2000. All rights reserved.
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
11.00 6. Tool Offsets and Compensation
Approach/exit contour, NORM/KONT
KONT G41 X... Y... Z...
G450
NORM The tool travels directly along a straight line
and is perpendicular to the contour point.
KONT The tool travels around the contour point in
accordance with
the programmed behavior at corners
G450/G451.
For KONT: If start point and contour point are on one side
of a workpiece, the contour point is approached as with
NORM directly along a straight line.
a = 1st contour point
Start
NORM G42...
KONT G42...
a
KONT G450 G42
a
Start
Programmable behavior for approach and exit
© Siemens AG 2000. All rights reserved. 6-47
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
6. Tool Offsets and Compensation 11.00
Move along the contour, G450/G451
N10 G41 X... Y... Z...
G450
G450 Transition circle, the tool travels around
workpiece corners
along a circular path with tool radius.
G451 Intersection point, the tool cuts free in the
workpiece corner.
a = Transition circle
b = Intersection point
G450
a
G451
b
Tool travel behavior at workpiece corners
6-48 © Siemens AG 2000. All rights reserved.
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
7. Coordinate Systems
Frame concept 7-50
Shift/rotate coordinates, TRANS/ROT 7-51
Mirroring the coordinate axes, MIRROR 7-52
Increasing/reducing size of contour, SCALE 7-53
© Siemens AG 2000. All rights reserved. 7-49
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
7. Coordinate Systems 11.00
Frame concept
For the three-dimensional description of the workpiece
coordinate system, the following functions are available.
TRANS/ATRANS Translation of the zero point
ROT/AROT Rotation
SCALE/ASCALE Change of scale
MIRROR/AMIRROR Mirroring
The actual coordinate system can be anywhere in space.
This also allows skew contours to be produced.
Z0
Y1
Z1
Y0
X1
X0
Programmable frames allow inclined contours to be machined
7-50 © Siemens AG 2000. All rights reserved.
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
11.00 7. Coordinate Systems
Shift/rotate coordinates, TRANS/ROT
N30 ... G54
N40 G90 TRANS X40 Y40 Z30
N50 G90 AROT Z30
To switch off ZO: TRANS (without specifying
axis)
To switch off rotation: ROT (without specifying angle)
In all cases, the complete frame is deleted here!
TRANS Absolute* offset
* additive to a possibly activated selectable
offset (G54  G59)
ATRANS (to a previously activated TRANS offset)
additive offset
X, Y, Z Coordinates of zero offset in axial direction
ROT Absolute rotation
AROT Additive rotation
X, Y, Z Coordinate axis about which rotation occurs in
angular degrees (positive sign = counter-
clockwise rotation)
TRANS X40 Y40 Z10 A30
AROT Z30
Z
G54 Y
Z
Y
Y
X
TRANS
AROT
X
X
Changing the zero point for producing a drilling pattern
© Siemens AG 2000. All rights reserved. 7-51
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
X
7. Coordinate Systems 11.00
Mirroring the coordinate axes, MIRROR
N10 MIRROR X0
Switch off MIRROR (without defining axis)
In all cases, the complete frame is deleted here!
MIRROR Absolute mirroring
AMIRROR Additive mirroring
X0, Y0, Z0 Address with value 0 of the axis at which
mirroring takes place.
When mirroring on a coordinate axis, the control changes
" the sign of the mirrored coordinates,
" the direction of rotation for circulate interpolation, and
" the machining direction (G41/G42).
Y
MIRROR X0
AMIRROR Y0
X
No additional programming for symmetrical contours
7-52 © Siemens AG 2000. All rights reserved.
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
11.00 7. Coordinate Systems
Increasing/reducing size of contour,
SCALE
N10 SCALE X2 Y2 Z2
Switch off SCALE (without defining axis)
In all cases, the complete frame is deleted here!
SCALE New scale factor
ASCALE Additive scale factor
X, Y, Z Axes with scale factor in the direction of which
the contour is to be increased or reduced in
size.
If transformation follows with ATRANS, the offset values are
also scaled.
Any contours that you wish to increase or reduce in size are
best defined in a subroutine.
You can define an individual scale factor for each axis.
SCALE X2 Y2 Z2
Z
Y
X
No additional programming for similar contours
© Siemens AG 2000. All rights reserved. 7-53
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
7. Coordinate Systems 11.00
7-54 © Siemens AG 2000. All rights reserved.
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
8. Programming Preparatory Functions
Exact stop, G9/G60 8-56
Feed in continuous path mode, G64 8-57
Programming the spindle motion 8-58
Subroutine technique 8-59
© Siemens AG 2000. All rights reserved. 8-55
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
8. Programming Preparatory Functions 11.00
Exact stop, G9/G60
G601 Exact positioning fine
G602 Exact positioning coarse
G9 Exact positioning, active in the block
G60 Exact positioning, modal, active until deselected by
G64, G641.
The exact positioning functions are used in order to
produce sharp outside corners or to finish inside corners to
the required dimension.
The exact positioning limits are defined in the machine
data.
Z
G602
G601
X
Producing sharp outside corners
8-56 © Siemens AG 2000. All rights reserved.
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
11.00 8. Programming Preparatory Functions
Feed in continuous path mode, G64
N05 ...
N10 G1 Z-7 F300
N20 G64
N30 Y40
G64 Continuous path mode
The function operates velocity look ahead function, i.e. the
path velocity is only reduced so that the mechanical
machine limit values are maintained.
G64
Optimization of the production results
© Siemens AG 2000. All rights reserved. 8-57
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
8. Programming Preparatory Functions 11.00
Programming the spindle motion
N05 ...
N10 G1 F300 X70 Y20 S270 M3
S Spindle speed in rpm
M3 Clockwise rotation
M4 Counter-clockwise rotation
M5 Spindle stop
If the M commands are programmed in a block with axial
motion, the commands before the axial motion are effective.
M3 M4
Programming the direction of spindle rotation
8-58 © Siemens AG 2000. All rights reserved.
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
11.00 8. Programming Preparatory Functions
Subroutine technique
N40 G0 X500 Y500 Z500
N50 L230 P2
L... Subroutine call
P... Number of repeats (max. 9999)
Maximum sub-routine nesting: 8x; i.e. an MPF can call up to
seven nested SPFs.
The end of the subroutine and the return jump to the main
program is programmed using M17 or RET. The subroutine
call must be realized in a dedicated NC block.
N40.........
N50 L230 P2
N5 G91 G00...
/.......
Z
N20 M17
Y
X
Machining in several steps
© Siemens AG 2000. All rights reserved. 8-59
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
8. Programming Preparatory Functions 11.00
8-60 © Siemens AG 2000. All rights reserved.
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
9. Attachment
List of M commands 9-62
List of G functions 9-63
Notes 9-68
© Siemens AG 2000. All rights reserved. 9-61
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
9. Attachment 11.00
List of M commands
M0* Programmed stop
M1* Optional stop
M2* End of program (main program)
M30* End of program as M2
M17* End of subroutine
M3 Spindle clockwise
M4 Spindle counter-clockwise
M5 Spindle stop
M6 Tool change
M70 Reserved for Siemens
M40 Automatic gear change
M41 Gear stage 1
M42 Gear stage 2
M43 Gear stage 3
M44 Gear stage 4
M45 Gear stage 5
The extended address notation is not permissible for the functions
designated with *.
Machine OEM
All free M function numbers can be assigned by the
machine manufacturer. For example, with switching
functions for controlling clamping devices or for
activating/de-activating further machine functions.
9-62 © Siemens AG 2000. All rights reserved.
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
11.00 9. Attachment
List of G functions
Group 1: Modal motion commands
Name No. Meaning m/n Def.
G0 1. Rapid traverse motion m
G1 2. Linear interpolation m Def.
G2 3. Circular interpolation clockwise m
G3 4. Circular interpolation counter-clockwise m
CIP 5. Circular interpolation through point m
G33 10. Thread cutting with constant lead m
G331 11. Rigid tapping m
G332 12. Return (rigid tapping) m
Group 2: Non-modal motion commands, dwell time
G4 1. Dwell time preset n
G63 2. Tapping without synchronization n
G74 3. Reference point approach with synchronization n
G75 4. Fixed point approach n
m: modal, n: non-modal, Def.: Default
© Siemens AG 2000. All rights reserved. 9-63
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
9. Attachment 11.00
List of G functions
Group 3: Write memory
Name No. Meaning m/n Def.
TRANS 1. TRANSLATION: translation, programmable n
ROT 2. ROTATION: rotation, programmable n
SCALE 3. SCALE: scaling, programming n
MIRROR 4. MIRROR: mirroring, programmable n
ATRANS 5. Additive translation, programmable n
AROT 6. Additive rotation, programmable n
ASCALE 7. Additive scaling, programming n
AMIRROR 8. Additive mirroring, programmable n
G25 10. Minimum working area limitation/spindle speed n
limitation
G26 11. Maximum working area limitation/spindle speed n
limitation
G110 12. Pole programming relative to the last n
programmed setpoint position
G111 13. Pole programming relative to the zero of the n
present WCS
G112 14. Pole programming relative to the last valid pole n
Group 6: Plane selection
G17 1. Plane selection 1st - 2nd geometry axis m Def.
milling
G18 2. Plane selection 3rd - 1st geometry axis m Def.
turnin
g
G19 3. Plane selection 2nd - 3rd geometry axis m
m: modal
n: non-modal
Def.: Default
9-64 © Siemens AG 2000. All rights reserved.
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
11.00 9. Attachment
List of G functions
Group 7: Tool radius compensation
Name No. Meaning m/n Def.
G40 1. No tool radius compensation m
G41 2. Tool radius compensation left of contour m
G42 3. Tool radius compensation right of contour m
Group 8: Settable zero offset
G500 1. Cancel G54 - G59, reset adjustable frame m Def.
G54 2. 1st settable zero offset m
G55 3. 2nd settable zero offset m
G56 4. 3rd settable zero offset m
G57 5. 4th settable zero offset m
G58 6. 5th settable zero offset m
G59 7. 6th settable zero offset m
Group 9: Frame suppression
G53 1. Suppresses current frame n
Suppresses the actual zero offset
SUPA 2.
Group 10: Exact stop, continuous path mode
G60 1. Velocity reduction, exact positioning m Def.
G64 2. Continuous path mode m
Group 11: Exact stop blockwise
G9 1. Velocity reduction, exact positioning n
m: modal
n: non-modal
Def.: Default
© Siemens AG 2000. All rights reserved. 9-65
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
9. Attachment 11.00
List of G functions
Group 12: Block change criteria at exact stop (G60/G09)
Name No. Meaning m/n Def.
G601 1. Block change at exact stop fine m Def.
G602 2. Block change at exact stop coarse m
Group 13: Workpiece dimensioning inch/metric
G70 1. Input system inch m
G71 2. Input system metric m Def.
Group 14: Workpiece dimensioning absolute/incremental
G90 1. Absolute dimension input m Def.
G91 2. Incremental dimension input m
Group 15: Feed rate type
G94 2. Linear feed mm/min, inch/min m Def.
milling
G95 3. Rotational feed in mm/rev, inch/rev m Def.
turnin
g
G96 4. Constant cutting velocity ON
G97 5. Constant cutting velocity OFF
Group 16: Feed correction (offset) at inner and outer curved surfaces *)
CFC 1. Constant feed at contour m Def.
CFTCP 2. Constant feed in tool center point m
CFIN 3. Constant feed at inside curvature m
m: modal
n: non-modal
Def.: Default
*)
the commands of this group are not described in this document
9-66 © Siemens AG 2000. All rights reserved.
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
11.00 9. Attachment
List of G functions
Group 18: Corner behavior, tool compensation
Name No. Meaning m/n Def.
G450 1. Transition circle m Def.
G451 2. Intersection of equidistances m
Group 21: Acceleration profile *)
BRISK 1. Fast non-smoothed path acceleration m Def.
SOFT 2. Soft smoothed path acceleration m
Group 24: Feed control *)
FFWOF 1. Feed forward control off m Def.
FFWON 2. Feed forward control on m
Group 28: Working area limiting, on/off *)
WALIMON 1. Working area limitation on m
WALIMOF 2. Working area limitation off m Def.
Group 29: Radius  Diameter *)
DIAMOF 1. Diameter programming off m Def.
DIAMON 2. Diameter programming on m
m: modal
n: non-modal
Def.: Default
*)
The commands of this group are not described in this document
© Siemens AG 2000. All rights reserved. 9-67
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
9. Attachment 11.00
Notes
You can enter your own user-specific functions here.
9-68 © Siemens AG 2000. All rights reserved.
SINUMERIK 802D Brief Instructions Milling (BNKF) - 11.00 Edition.
Suggestions
To:
Corrections
SIEMENS AG
A&D MC BMS for Publication/Manual:
SINUMERIK 802D
P.O. Box 3180
Milling
D-91050 Erlangen
(Tel. 0180 / 525 - 8008 / 5009 [Hotline]
Fax [phone] / 98 - 2176
email: motioncontrol.docu@.siemens.de) User Documentation
From Milling
Order No.: 6FC5298-1AA40-0BP0
Name
Edition: 11.00
Company/Dept. Should you come across any printing
errors when reading this publication,
Address
please notify us on this sheet.
_____________________________________
Suggestions for improvement are also
welcome.
_____________________________________
Telephone /
_____________________________________
Telefax: /
Suggestions and/or corrections