SINUMERIK 840D sl/828D. Job Planning. Programming Manual (2010-2018)

Additional functions

18.2 Replaceable geometry axes (GEOAX)

18.2

Replaceable geometry axes (GEOAX)

The "Switchable geometry axes" function allows the geometry axes configured via machine

data to be replaced by other channel axes.

Syntax

GEOAX(<n>,<channel axis>,<n>,<channel axis>,<n>,<channel axis>)

GEOAX()

Meaning

GEOAX(...)

Function for switching geometry axes.

Note:

GEOAX() without parameter specification activates the basic configuration of

the geometry axes parameterized in the machine data again.

<n>

Number of the geometry axis that is to be replaced by the specified channel axis.

Range of values:

0, 1, 2, 3

Note:

0: The specified channel axis is removed from the geometry axis group without

being replaced

1: 1. geometry axis ≙ coordinate axis X (abscissa) of the WCS

2: 2. geometry axis ≙ coordinate axis Y (ordinate) of the WCS

3: 3. geometry axis ≙ coordinate axis Z (applicate) of the WCS

Name of the channel axis which is to added to the geometry axis group

Examples

Example 1: Switching two axes alternating as geometry axis

A tool slide can be traversed using channel axes X1, Y1, Z1, Z2:

Job Planning

628

Programming Manual, 12/2018, A5E40869460B AB

Additional functions

18.2 Replaceable geometry axes (GEOAX)

;

The geometry axes are configured so that after powering-up, initially Z1 is effective as 3rd

geometry axis under the geometry axis name "Z" and together with X1 and Y1 forms the

geometry axis group.

Axes Z1 and Z2 should now be used, alternating, as geometry axis Z in the part program:

Program code

Comment

N100 GEOAX(3,Z2)

; Channel axis Z2 acts as 3rd geometry axis (Z).

N110 G1 ...

N120 GEOAX(3,Z1)

; Channel axis Z1 acts as 3rd geometry axis (Z).

Example 2: Changing over the geometry axes for six channel axes

A machine has six channel axes with the names XX, YY, ZZ, U, V, W.

The basic setting of the geometry axis configuration via machine data is:

Channel axis XX = 1st geometry axis (X axis)

Channel axis YY = 2nd geometry axis (Y axis)

Channel axis ZZ = 3rd geometry axis (Z axis)

Program code

Comment

N10 GEOAX()

; The basic configuration of the geometry axes is ef-

fective.

N20 G0 X0 Y0 Z0 U0 V0 W0

; All axes in rapid traverse to position 0.

N30 GEOAX(1,U,2,V,3,W)

; Channel axis U becomes the first (X), V the second

(Y)

; and W the third geometry axis (Z).

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

629

Additional functions

18.2 Replaceable geometry axes (GEOAX)

Program code

Comment

N40 GEOAX(1,XX,3,ZZ)

; Channel axis XX becomes the first (X), ZZ the third

; geometry axis (Z). Channel axis V remains the second

; geometry axis (Y).

N50 G17 G2 X20 I10 F1000

; Full circle in the X/Y plane. Channel axes

; XX and V traverse.

N60 GEOAX(2,W)

; Channel axis W becomes the second geometry (Y).

N80 G17 G2 X20 I10 F1000

; Full circle in the X/Y plane. Channel axes

; XX and W traverse.

N90 GEOAX()

; Reset to the initial state.

N100 GEOAX(1,U,2,V,3,W)

; Channel axis U becomes the first (X), V the second

; (Y) and W the third geometry axis (Z).

N110 G1 X10 Y10 Z10 XX=25

; Channel axes U, V, W each traverse to

; position 10. XX as special axis traverses to posi-

tion 25.

N120 GEOAX(0,V)

; V is removed from the geometry axis group.

; U and W remain the first (X) and third

; geometry axis (Z).

; The second geometry (Y) axis remains unassigned.

N130 GEOAX(1,U,2,V,3,W)

; Channel axis U remains the first (X), V becomes

; the second (Y), W remains the third geometry axis

(Z).

N140 GEOAX(3,V)

; V becomes the third geometry axis (Z), whereby W

; is overwritten and therefore removed from the geom-

etry

; axis group. The second geometry axis (Y)

; still remains unassigned.

Machine data

Axis configuration

Assignment of geometry, special and machine axes to channel axes:

● MD10000 $MN_AXCONF_MACHAX_NAME_TAB

● MD20050 $MC_AXCONF_GEOAX_ASIGN_TAB

● MD20060 $MC_AXCONF_GEOAX_NAME_TAB

● MD20070 $MC_AXCONF_MACHAX_USED

● MD20080 $MC_AXCONF_CHANAX_NAME_TAB

● MD35000 $MA_SPIND_ASSIGN_TO_MACHAX

Reset behavior

Reset behavior of changed geometry axis assignments:

● MD20110 $MC_RESET_MODE_MASK, bit 12

● MD20118 $MC_GEOAX_CHANGE_RESET

Job Planning

630

Programming Manual, 12/2018, A5E40869460B AB

Additional functions

18.2 Replaceable geometry axes (GEOAX)

NC start behavior

● MD20112 $MC_START_MODE_MASK, bit 12

Notification to the PLC user program

Parameterization option of the M command which is output on the NC/PLC interface when the

geometry axes are changed.

● MD22532 $MC_GEOAX_CHANGE_M_CODE

Supplementary conditions

No geometry axis changeover

● If one of the following functions is active, a geometry axis changeover is not possible:

- Transformation

- Spline interpolation

- Tool radius compensation

- Tool fine offset

● The geometry axis and another channel axis have the same name.

● One of the axes participating in the geometry axis changeover is involved in an action that

goes beyond block limits, e.g. block-wide positioning axis or following axis of an axis

coupling.

Rotary axes

Rotary axes cannot be programmed as geometry axes.

Axis state after replacing

An axis replaced by the changeover in the geometry axis group can be programmed as

supplementary axis after the changeover operation via its channel axis names.

Frames, protection areas, working area limits

All frames, protection areas and working area limits are deleted after changing over the

geometry axes.

Polar coordinates

Replacing the geometry axes with GEOAX sets analog to a level change with G17-G19, the

modal polar coordinates to a value of 0.

DRF, WO

A possible handwheel offset (DRF) or an external work offset (WO) remains effective after the

changeover.

Basic configuration of the geometry axes

The GEOAX() command calls the basic configuration of the geometry axis group.

The system automatically changes back to the basic configuration after POWER ON and when

changing over into the "reference point approach" mode.

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

631

Additional functions

18.2 Replaceable geometry axes (GEOAX)

Tool length compensation

An active tool length compensation is also effective after the changeover operation. However,

for geometry axes that have been newly added or those where the position has been replaced,

it is still considered not to have been moved through. For the first motion command for these

geometry axes, the resulting traversing distance correspondingly comprises the sum of the

tool length compensation and the programmed traversing distance.

Geometry axes, which retain their position in the axis group after a replacement operation,

also retain their status with respect to tool length compensation.

Geometry axis configuration for active transformation

● The geometry axis configuration parameterized for an active transformation via

transformation machine data cannot be changed using the "Switchable geometry axes"

function.

● Different data sets must be parameterized in the transformation machine data for a different

geometry axis configuration for a transformation.

● A geometry axis configuration changed using GEOAX is deleted by activating a

transformation.

● With regard to the geometry axes, the transformation-specific geometry axis

parameterizations of active transformations have priority over the parameterizations

relevant for the changeover of geometry axes.

Example: A transformation is active. According to the machine data, the transformation

should be retained at a channel reset. At the same time, the basic configuration of the

geometry axes should be restored at a channel reset. The geometry axis configuration that

has been specified for the transformation is retained.

● If a transformation is switched off, the parameterized basic setting of the geometry axis

configuration takes effect again.

JOG mode, REF machine function

When switching over to the JOG mode, REF machine function (reference point approach), the

geometry axis configuration parameterized in the machine data takes effect

Job Planning

632

Programming Manual, 12/2018, A5E40869460B AB

Additional functions

18.3 Axis container (AXCTSWE, AXCTSWED, AXCTSWEC)

18.3

Axis container (AXCTSWE, AXCTSWED, AXCTSWEC)

The "AXCTSWE" or "AXCTSWED" commands enable the rotation of the specified axis

container.

Any previously set enable for axis container rotation is cancelled with the "AXCTSWEC"

command.

Syntax

AXCTSWE(<ID>)

AXCTSWED(<ID>)

AXCTSWEC(<ID>)

Meaning

AXCTSWE:

Enable for rotation of the axis container

The program processing is not stopped by "AXCTSWE".

The rotation is performed as soon as all channels involved on the axis container have

been enabled.

AXCTSWED:

Enable to rotate the axis container without consideration of the other channels in-

volved on the axis container

Note

● Command variant to simplify the commissioning of the part program or

synchronized action.

● The behavior with regard to the other channels involved on axis container can be

specified via:

MD12760 $MN_ AXCT_FUNCTION_MASK, bit 0

AXCTSWEC:

Canceling the enable to rotate the axis container

Note

The enable for rotating an axis container can only be cancelled when the rotation

has yet not been started:

$AN_AXCTSWA[<axis container>] == 0

For system variable, see "Axis container (AXCTSWE, AXCTSWED, AXCTSWEC)

(Page 633)"

<ID>:

Identifier of the axis container or a container axis:

CT<number>:

Default identifier of an axis container:

MD12750 $MN_AXCT_NAME_TAB

Example: "CT1"

<Container>:

User-specific identifier of an axis container:

MD12750 $MN_AXCT_NAME_TAB

Example: "CONTAINER_1"

<axis>:

Identifier of a known container axis in the channel

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

633

Additional functions

18.3 Axis container (AXCTSWE, AXCTSWED, AXCTSWEC)

Note

Increment

The increment of a axis container rotation is set via the setting data:

SD41700 $SN_AXCT_SWWIDTH

Further information

Diagnostics

The current status of a axis container can be read via the following system variables:

System variable

Type

Description

$AC_AXCTSWA[<name>]

BOOL

Channel-specific status of the axis container

$AN_AXCTSWA[<axis container>]

BOOL

NCU-specific status of the axis container

$AN_AXCTSWE[<axis container>]

INT

Slot-specific status of the axis container rotation

The system variable supplies the status of the axis

container slot bitwise. Each bit corresponds to a

slot.

$AN_AXCTAS[<axis container>]

INT

Number of locations (slots) through which the axis

container was just switched through.

Axis container rotation with implicit GET / GETD

The following machine data can be use to set that all container axes of the channel are brought

into the channel by means of an implicit "GET/GETD" with the "AXCTSWE" command. An axis

replacement is only possible again after the container rotation.

MD10722 $MN_AXCHANGE_MASK, bit 1 = 1

Note

An axis container rotation with implicit "GET/GETD" is not performed for an axis in the state

"main run axis" (e.g. PLC axis) because the axis would have to exit the state for the axis

container rotation.

Job Planning

634

Programming Manual, 12/2018, A5E40869460B AB

Additional functions

18.4 Wait for valid axis position (WAITENC)

18.4

Wait for valid axis position (WAITENC)

Using the language command "WAITENC", the NC program waits until the synchronized or

restored axis positions are available for the axes configured with

MD34800 $MA_WAIT_ENC_VALID = 1.

An interruption can take place in the wait state, e.g. by starting an ASUB or by changing the

operating mode to JOG. When the program is continued, where relevant, the wait state is

resumed.

Note

In the user interface, the wait state is displayed using the hold state "Wait for measuring

system".

Syntax

"WAITENC" can be programmed in the program section of any NC program.

Programming must be realized in a dedicated block:

WAITENC

Example

"WAITENC" is for example used in an event-controlled user program, .../_N_CMA_DIR/

_N_PROG_EVENT_SPF, as shown in the following application example.

Application example: Tool withdrawal after POWER OFF with orientation transformation

Machining with tool orientation was interrupted due to a power failure.

When powering up again, the event-controlled user program .../_N_CMA_DIR/

_N_PROG_EVENT_SPF is called.

In the event-controlled user program, the system waits for synchronized or restored axis

positions using "WAITENC"; in order to then be able to calculate a frame, which aligns the

Work in the tool direction.

Program code

Comment

IF $P_PROG_EVENT == 4

; Run-up.

IF $P_TRAFO <> 0

; Transformation has been selected.

WAITENC

; Wait for valid axis positions of the orientation

axes.

TOROTZ

; Rotate the Z axis of the WCS towards the tool axis.

ENDIF

M17

ENDIF

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

635

Additional functions

18.5 Programmable parameter set changeover (SCPARA)

18.5

Programmable parameter set changeover (SCPARA)

The changeover to a specific parameter set can be requested for an axis with the SCPARA

command.

Note

No parameter set changeover during thread cutting

During thread cutting G33 and tapping G331/G332, the parameter set is selected by the control

and cannot be changed.

Disabled parameter set changeover

A parameter set changeover can also be requested via the NC/PLC interface. In order to avoid

changeover conflicts, the parameter set changeover of the NC (SCPARA) can be disabled via

the NC/PLC interface:

DB31, ... DBX9.3 (parameter set specification disabled by NC)

Note

If a parameter set changeover is requested by SCPARA while the parameter set changeover

is disabled via the NC/PLC interface, the changeover is rejected without an error message.

Syntax

SCPARA[<axis>]=<value>

Meaning

SCPARA:

Command: Change parameter set

<axis>:

Axis identifier (channel axis)

Type:

AXIS

<value>:

Parameter set number: 1, 2, 3, ... max. parameter set number

Example

Program code

Comment

N110 SCPARA[X]= 3

; Select: Axis X, 3rd parameter set

Further information

Enable of the parameter set changeover

The parameter set changeover of the axis must be explicitly enabled:

MD35590 $MA_PARAMSET_CHANGE_ENABLE[<axis>]

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

637

Additional functions

18.6 Check scope of NC language present (STRINGIS)

18.6

Check scope of NC language present (STRINGIS)

Using the function "STRINGIS(...)" it can be checked as to whether the specified string is

available as element of the NC programming language in the actual language scope.

Definition

INT STRINGIS(STRING <Name>)

Syntax

STRINGIS(<Name>)

Meaning

STRINGIS:

Function with return value

<name>:

Name of the NC programming language element to be checked

Return value:

The return value format is yxx (decimal).

Elements of the NC programming language

The following elements of the NC programming language can be checked:

● G commands of all existing G groups, e.g. "G0", "INVCW", "POLY", "ROT", "KONT",

"SOFT", "CUT2D", "CDON", "RMBBL", "SPATH"

● DIN or NC addresses, such as "ADIS", "RNDM", "SPN", "SR", "MEAS"

● Functions, e.g. "TANG(...)" or "GETMDACT"

● Procedures, e.g. "SBLOF".

● Keywords, e.g. "ACN", "DEFINE" or "SETMS"

● System data, e.g. machine data $M... , setting data $S... or option data $O...

● System variables $A... , $V... , $P...

● Arithmetic parameter R...

● Cycle names of activated cycles

● GUD and LUD variables

● Macro names

● Label names

Return value

Only the first three decimal positions of the return value are relevant. The return value format

is yxx, with y = basis information and xx = detailed information.

Return value

Meaning

000

The 'name' string is not known in this system ¹⁾

100

The 'name' string is an element of the NC programming language, but currently cannot be programmed

(option/function is inactive)

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

639

Additional functions

18.6 Check scope of NC language present (STRINGIS)

Return value

Meaning

2xx

The 'name' string is a programmable element of the NC programming language (option/function is active).

The detailed information xx contains additional information about the element type:

Meaning

DIN address or NC address²⁾

G command (e.g. G04, INVCW)

Function with return value

Function without return value

Keyword, e.g. DEFINE

Machine ($M...), setting ($S...) or option data ($O...)

System parameters, e.g. system variable ($...) or arithmetic parameter (R...)

Cycle (the cycle must be loaded into the NC and the cycle program must be active ³⁾ )

GUD variable (the GUD variable must be defined in the GUD definition files and the GUD variables

activated)

Macro name (the macro must be defined in the macro definition files and macros activated) ⁴⁾

LUD variable of the actual part program

ISO G command (ISO language mode must be active)

400

The 'name' string is an NC address, that was not identified as xx == 01 or xx == 10 and is not G or R ²⁾

y00

No specific assignment possible

1) Depending on the control, under certain circumstances, only a subset of the Siemens NC language commands are known,

e.g. SINUMERIK 802D sl. For these controls, for strings that are principally Siemens NC language commands, a value of 0

is returned. This behavior can be changed using MD10711 $MN_NC_LANGUAGE_CONFIGURATION. For MD10711 = 1,

then a value of 100 is always returned for Siemens NC language commands.

2) NC addresses are the following letters: A, B, C, E, I, J, K, Q, U, V, W, X, Y, Z. These NC addresses can also be programmed

with an address extension. The address extension can be specified when checking with STRINGIS. Example: 201 ==

STRINGIS("A1").

The letters: D, F, H, L, M, N, O, P, S, T are NC addresses or auxiliary functions that are defined by the user. A value of 400

is always returned for these. Example: 400 == STRINGIS( "D" ). These NC addresses cannot be specified with address

extension when checking with STRINGIS.

Example: 000 == STRINGIS("M02"), but 400 == STRINGIS("M").

3) Names of cycle parameters cannot be checked with STRINGIS.

4) Address, defined as macro, e.g. G, H, M, L are identified as macro.

Examples

In the following examples it is assumed that the NC language elements specified as string -

as long as nothing else is noted - can in principle be programmed in the control.

1. String "T" is defined as auxiliary function:

400 == STRINGIS("T")

000 == STRINGIS ("T3")

2. String "X" is defined as axis:

201 == STRINGIS("X")

201 == STRINGIS("X1")

3. String "A2" is defined as address with extension:

201 == STRINGIS("A")

201 == STRINGIS("A2")

4. String "INVCW" is defined as named G command:

202 == STRINGIS("INVCW")

Job Planning

640

Programming Manual, 12/2018, A5E40869460B AB

Additional functions

18.6 Check scope of NC language present (STRINGIS)

5. String "$MC_GCODE_RESET_VALUES" is defined as machine data:

206 == STRINGIS("$MC_GCODE_RESET_VALUES")

6. String "GETMDACT" is an NC language function:

203 == STRINGIS("GETMDACT ")

7. String "DEFINE" is a keyword:

205 == STRINGIS("DEFINE")

8. String "$TC_DP3" is a system parameter (tool length component):

207 == STRINGIS("$TC_DP3")

9. String "$TC_TP4" is a system parameter (tool size):

207 == STRINGIS("$TC_TP4")

10.String "$TC_MPP4" is a system parameter (magazine location state):

- Tool magazine management is active: 207 == STRINGIS("$TC_MPP4") ;

- Tool magazine management is not active: 000 == STRINGIS("$TC_MPP4")

Also refer to the paragraph below: Tool magazine management.

11.String "MACHINERY_NAME" is defined as GUD variable:

209 == STRINGIS("MACHINERY_NAME")

12.String "LONGMACRO" is defined as macro:

210 == STRINGIS("LONGMACRO")

13.String "MYVAR" is defined as LUD variable:

211 == STRINGIS("MYVAR")

14.String "XYZ" is a command that is not known in the NC, GUD variable, macro or cycle name:

000 == STRINGIS("XYZ")

Tool magazine management

If the tool magazine management function is not active, supplies STRINGIS for the system

parameters of the tool magazine management, independent of the machine data

● MD10711 $MN_NC_LANGUAGE_CONFIGURATION

always a value of 000.

ISO mode

If the "ISO mode" function is active:

● MD18800 $MN_MM_EXTERN_LANGUAGE (activation, external NC languages)

● MD10880 $MN_ MM_EXTERN_CNC_SYSTEM (control system to be adapted)

STRINGIS checks the specified string initially as SINUMERIK G command. If the string is not

a SINUMERIK G command, then it is subsequently checked as ISO G command.

Programmed switchovers (G290 (SINUMERIK mode), G291 (ISO Mode)) have no effect on

STRINGIS.

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

641

Additional functions

18.6 Check scope of NC language present (STRINGIS)

Example

The machine data, relevant for the function STRINGIS(...), has the following values:

● MD10711 $MN_NC_LANGUAGE_CONFIGURATION = 2 (only the NC language

commands whose options are set are considered to be known)

● MD19410 $ON_TRAFO_TYPE_MASK = 'H0' (option: transformations)

● MD10700 $MN_PREPROCESSING_LEVEL='H43' (preprocessing for cycles is active)

The following program example is executed without error message:

Program code

Comment

N1 R1=STRINGIS("TRACYL")

; R1 == 0, because TRACYL is identified as

"not known" because of the missing transformation

option

N2 IF STRINGIS("TRACYL") == 204

N3 TRACYL(1,2,3)

; N3 is skipped

N4 ELSE

N5 G00

; and instead, N5 is executed

N6 ENDIF

N7 M30

Job Planning

642

Programming Manual, 12/2018, A5E40869460B AB

Additional functions

18.7 Interactively call the window from the part program (MMC)

18.7

Interactively call the window from the part program (MMC)

Via the predefined subprogram MMC(...), user-specific dialogs can be displayed from an NC

program on the user interface of SINUMERIK Operate, for example.

The configuration of the dialogs can be done for the following types of dialogs:

● Run MyScreens

● Easy XML

● User XML

References

● Programming Manual Run MyScreens

● Programming Manual Easy XML

Syntax

MMC("<ADDRESS>,<COMMAND>,<FILE>,<DIALOG>","<QUIT>")

Meaning

MMC(...):

Subprogram identifier

The parameters are specified position-coded and separated by a comma

within two strings, the command string and the acknowledgement string.

Parameters within the command string:

<ADDRESS>:

Operating area in which the configured user dialog boxes are implemented

Function

Operating areas

"Run MyScreens" user dialog

CYCLES

"Easy XML" user dialog

CYCLES

User XML

XML

Pop-up window "Run MyScreens"

POPUPDLG

Popup window "Easy XML"

POPUPDLG

<COMMAND>:

Command to be executed

Function

Commands

"Run MyScreens" user dialog

PICTURE_ON, PICTURE_OFF

"Easy XML" user dialog

PICTURE_ON, PICTURE_OFF

User XML

XML_ON, XML_OFF

Pop-up window "Run MyScreens"

PICTURE_ON, PICTURE_OFF

Popup window "Easy XML"

PICTURE_ON, PICTURE_OFF

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

643

Additional functions

18.7 Interactively call the window from the part program (MMC)

<FILE>:

Name of the file in which the dialog to be displayed is programmed

Function

Files

"Run MyScreens" user dialog

<name>.com

"Easy XML" user dialog

<name>.xml

User XML

<name>.xml

Pop-up window "Run MyScreens"

<name>.com

Popup window "Easy XML"

<name>.xml

Popup window "Easy XML" with configura-

xmldial_emb.xml

tion direct in the NC program (see example

<DIALOG>:

Name of the dialog to be displayed

Function

Dialog name

All functions except popup window "Easy

Name of the dialog configured

XML" with configuration direct in the NC

in the <FILE> file

program

Popup window "Easy XML" with configura-

main

tion direct in the NC program (see example

Parameters within the acknowledgment string:

<QUIT>:

Acknowledgment type

No acknowledgment.

Program execution is continued when the command has been

transmitted. There is no feedback if the command could not be

successfully executed.

Note

Acknowledgement type "N" must be used if a display time (dwell

time) is programmed in the NC program (see Example 2 below)

Asynchronous acknowledgment

The program execution is continued after the command is issued.

The return value is saved in a user-specific acknowledgement

variable (GUD variable), which is defined within the scope of the

dialog configuration, and can be read in the NC program.

Example

Example 1

Display of a dialog and response to the user operation in an NC program.

Program code

Comment

; The acknowledgement variable QUIT has already been created as a global user varia-

ble (GUD)

; Of the type STRING when the dialog was configured:

; DEF NCK STRING[20] QUIT

QUIT = "XXX"

; Initialize acknowledgment variable

G4 F5

Job Planning

644

Programming Manual, 12/2018, A5E40869460B AB

Additional functions

18.7 Interactively call the window from the part program (MMC)

Program code

Comment

MMC("CYCLES,PIC-

; Display dialog

TURE_ON,test.com,test1","A")

;

- Operating area: CYCLES

;

- Picture status: PICTURE_ON (display)

;

- Dialog screen file: test.com

;

- Dialog screen: test1

INPUT:

; Wait for user input

STOPRE

;

Preprocessing stop

IF MATCH (QUIT,"RUN") >= 0 GOTOF WORK

;

Softkey "RUN"

IF MATCH (QUIT,"CHK") >= 0 GOTOF CHECK

;

Softkey "CHK"

GOTOB INPUT

; => Wait

WORK:

; Softkey "RUN" pressed

MSG("Continue with processing -> NC

; Output message

start")

MMC("CYCLES,PICTURE_OFF","N")

; Close dialog

; Wait for NC start

GOTOF END

; => Program end

CHECK:

; Softkey "CHK" pressed

MSG("Approach position -> NC start")

; Output message

MMC("CYCLES,PICTURE_OFF","N")

; Close dialog

; Wait for NC start

GOTOF END

; => Program end

END:

Example 2

The display time of a dialog is defined in the NC program via a dwell time, for example.

Program code

Comment

F1000 G94

MMC("POPUPDLG,PICTURE_ON,xmldial_emb.xml,main","N")

; Display dialog

X200

Z40

MMC("POPUPDLG,PICTURE_OFF","N")

; Close dialog

Example 3

Embedding a popup script in an NC program and its use.

Program code

PROC POPUP_TEST

; ----------------------------- Script -----------------------------

; <main_dialog entry="rpara_main">

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

645

Additional functions

18.7 Interactively call the window from the part program (MMC)

Program code

;

;

;

;

;

;

<open_form name="rpara_form"/>

;

<softkey_back>

;

<close_form />

;

</softkey_back>

;

</menu>

;

;

<init>

;

<caption>mask from NC part program</caption>

;

;

<op>

;

xpos = 120;

;

ypos = 34;

;

"nck/Channel/Parameter/R[10]" = 10;

;

</op>

;

;

<op>

;

num = "nck/Channel/Parameter/R[10]";

;

</op>

;

<while>

;

<condition> count < num</condition>

;

<print name="field_name" text="edit%d">count</print>

;

<op>

;

ypos = ypos + 24;

;

count = count + 1;

;

</op>

;

</while>

;

</init>

;

<paint>

;

<op>

;

xpos =

;

ypos = 36;

;

count = 0;

;

</op>

;

<while>

;

<condition>count < num</condition>

;

<print name="field_name" text="R-Parameter%d">count</print>

;

<text xpos = "$xpos" ypos = "$ypos" >$$$field_name</text>

;

<op>

;

ypos = ypos + 24;

Job Planning

646

Programming Manual, 12/2018, A5E40869460B AB

Additional functions

18.7 Interactively call the window from the part program (MMC)

Program code

;

count = count + 1;

;

</op>

;

</while>

;

</paint>

;

</form>

; </main_dialog>

; ========================= Program section ===========================

G94 F100

MMC("POPUPDLG,PICTURE_ON,xmldial_emb.xml,main","N")

G4 F4

X200

MMC("POPUPDLG,PICTURE_OFF","N")

G4 F2

Supplementary conditions

● The definition files *.com of the dialogs must be saved in the "proj" folder.

● The Easy XML definition files *.xml of the dialogs must be saved in the "appl" folder.

If the definition files are saved in a different directory, the path must be specified indirectly,

starting from the "appl" directory.

● User-defined dialogs cannot be simultaneously displayed from different channels.

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

647

Additional functions

18.8 Program runtime/part counter

18.8

Program runtime/part counter

Information on the program runtime and workpiece counter are provided to support the

machine tool operator.

This information can be processed as system variables in the NC and/or PLC program. This

information is also available to be displayed on the operator interface.

18.8.1

Program runtime

The "program runtime" function provides internal NC timers to monitor technological

processes, which can be read into the part program and into synchronized actions via the NC

and channel-specific system variables.

The trigger for the runtime measurement ($AC_PROG_NET_TIME_TRIGGER) is the only

system variable of the function that can be written to - and is used to selectively measure

program sections. This means, by writing $AC_PROG_NET_TIME_TRIGGER in the NC

program, the time measurement can be enabled and disabled again:

System variable

Meaning

Activity

NC-specific

$AN_SETUP_TIME

Time since the last control power up with default values

● Always active

("cold restart") in minutes.

Is automatically reset to "0" every time the control pow-

ers up with default values.

$AN_POWERON_TIME

Time since the last normal control power up ("warm

restart") in minutes.

Is automatically reset to "0" every time the control pow-

ers up normally.

Channel-specific

$AC_OPERATING_TIME

Total runtime of NC programs in automatic mode in

● Activated via

seconds.

MD27860

The value is automatically reset to "0" every time the

● Only AUTOMATIC

control powers up.

mode

$AC_CYCLE_TIME

Runtime of the selected NC program in seconds.

The value is automatically reset to "0" every time a new

NC program starts up.

$AC_CUTTING_TIME

Processing time in seconds

The runtime of the path axes (at least one is active) is

measured in all NC programs between NC start and

end of program/NC reset without rapid traverse active.

The measurement is interrupted when a dwell time is

active.

The value is automatically reset to "0" every time the

control powers up with default values.

Job Planning

648

Programming Manual, 12/2018, A5E40869460B AB

Additional functions

18.8 Program runtime/part counter

System variable

Meaning

Activity

$AC_ACT_PROG_NET_TIME

Actual net runtime of the current NC program in sec-

●

Always active

onds.

●

Only AUTOMATIC

Is automatically reset to "0" when a new NC program

mode

starts.

$AC_OLD_PROG_NET_TIME

Net runtime in seconds of the program that has just be

correctly ended with M30

$AC_OLD_PROG_NET_TIME_COUNT

Changes to $AC_OLD_PROG_NET_TIME

After POWER ON,

$AC_OLD_PROG_NET_TIME_COUNT is at "0".

$AC_OLD_PROG_NET_TIME_COUNT is always in-

creased if the control has newly written to

$AC_OLD_PROG_NET_TIME.

$AC_PROG_NET_TIME_TRIGGER

Trigger for the runtime measurement:

●

Only AUTOMATIC

Neutral state

mode

The trigger is not active.

Exit

Ends the measurement and copies the value from

$AC_ACT_PROG_NET_TIME into

$AC_OLD_PROG_NET_TIME.

$AC_ACT_PROG_NET_TIME is set to "0" and

then continues to run.

Start

Starts the measurement and in so doing sets

$AC_ACT_PROG_NET_TIME to "0".

$AC_OLD_PROG_NET_TIME is not changed.

Stop

Stops the measurement. Does not change

$AC_OLD_PROG_NET_TIME and keeps

$AC_ACT_PROG_NET_TIME constant until it re-

sumes

Resume

The measurement is resumed, i.e. a measure-

ment that was previously stopped is continued.

$AC_ACT_PROG_NET_TIME continues.

$AC_OLD_PROG_NET_TIME is not changed.

All system variables are reset to 0 as a result of POWER ON!

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

649

Additional functions

18.8 Program runtime/part counter

Note

Machine manufacturer

Machine data MD27860 $MC_PROCESSTIMER_MODE is used to switch-in the timer that can

be activated.

The behavior of active time measurements for certain functions (e.g. GOTOS, override = 0%,

active test run feed, program test, ASUB, PROG_EVENT, …) is configured using machine

data MD27850 $MC_PROG_NET_TIMER_MODE and

MD27860 $MC_PROCESSTIMER_MODE.

References:

Function Manual, Basic Functions; BAG, Channel, Program Operation, Reset Response (K1),

Chapter: Program runtime

Note

Residual time for a workpiece

If the same workpieces are machined one after the other, using the following timer values, the

remaining residual time for a workpiece can be determined.

● Processing time for the last workpiece produced (see $AC_OLD_PROG_NET_TIME)

● Current processing time (see $AC_ACT_PROG_NET_TIME)

The residual time is displayed on the user interface in addition to the current processing time.

Note

Using STOPRE

The system variables $AC_OLD_PROG_NET_TIME and

$AC_OLD_PROG_NET_TIME_COUNT do not generate any implicit preprocessing stop. This

is uncritical when used in the part program if the value of the system variables comes from the

previous program run. However, if the trigger for the runtime measurement

($AC_PROG_NET_TIME_TRIGGER) is written very frequently and as a result

$AC_OLD_PROG_NET_TIME changes very frequently, then an explicit STOPRE should be

used in the part program.

Supplementary conditions

● Block search

No program runtimes are determined through block searches.

● REPOS

The duration of a REPOS process is added to the current processing time

($AC_ACT_PROG_NET_TIME).

Job Planning

650

Programming Manual, 12/2018, A5E40869460B AB

Additional functions

18.8 Program runtime/part counter

Examples

Example 1: Measuring the duration of "mySubProgrammA"

Program code

N50 DO $AC_PROG_NET_TIME_TRIGGER=2

N60 FOR ii= 0 TO 300

N70 mySubProgrammA

N80 DO $AC_PROG_NET_TIME_TRIGGER=1

N95 ENDFOR

N97 mySubProgrammB

N98 M30

After the program has processed line N80, the net runtime of "mySubProgrammA" is located

in $AC_OLD_PROG_NET_TIME.

The value from $AC_OLD_PROG_NET_TIME:

● is kept beyond M30.

● is updated each time the loop is run through.

Example 2: Measuring the duration of "mySubProgrammA" and "mySubProgrammC"

Program code

N10 DO $AC_PROG_NET_TIME_TRIGGER=2

N20 mySubProgrammA

N30 DO $AC_PROG_NET_TIME_TRIGGER=3

N40 mySubProgrammB

N50 DO $AC_PROG_NET_TIME_TRIGGER=4

N60 mySubProgrammC

N70 DO $AC_PROG_NET_TIME_TRIGGER=1

N80 mySubProgrammD

N90 M30

18.8.2

Workpiece counter

The "Workpiece counter" function makes available various counters which can be used in

particular internally in the control to count workpieces.

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

651

Additional functions

18.8 Program runtime/part counter

The counters exist as channel-specific system variables with read and write access in a range

of values from 0 to 999 999 999.

System variable

Meaning

$AC_REQUIRED_PARTS

Number of workpieces to be produced (setpoint number of workpieces)

In this counter the number of workpieces at which the actual workpiece

count ($AC_ACTUAL_PARTS) will be reset to "0" can be defined.

$AC_TOTAL_PARTS

Total number of completed workpieces (actual workpiece total)

This counter specifies the total number of all workpieces produced since

the start time. The value is only automatically reset to "0" when the

control powers up with default values.

$AC_ACTUAL_PARTS

Number of completed workpieces (actual workpiece total)

This counter registers the total number of all workpieces produced since

the start time. On condition that $AC_REQUIRED_PARTS > 0, the

counter is automatically reset to "0" when the required number of work-

pieces ($AC_REQUIRED_PARTS) is reached.

$AC_SPECIAL_PARTS

Number of workpieces selected by the user

This counter supports user-specific workpiece counts. An alarm can be

defined to be output when the setpoint number of workpieces is reached

($AC_REQUIRED_PARTS). Users must reset the counter themselves.

Note

All workpiece counters are set to "0" when the control powers up with default values and can

be read and written independent of their activation.

Note

Channel-specific machine data can be used to control counter activation, counter reset timing

and the counting algorithm.

Note

Workpiece counting with user-defined M command

Machine data can be set so that the count pulses for the various workpiece counters are

triggered using user-defined M commands rather than the end of the program (M2/M30).

Job Planning

652

Programming Manual, 12/2018, A5E40869460B AB

Additional functions

18.9 Process DataShare - Output to an external device/file (EXTOPEN, WRITE, EXTCLOSE):

18.9

Process DataShare - Output to an external device/file (EXTOPEN,

WRITE, EXTCLOSE):

The writing of data from a part program to an external device/file is performed in three steps:

1. Open the external device/file

The external device/file is opened for the channel for writing using the EXTOPEN command.

2. Writing data

The output data can be processed using the string functions of the NC language, e.g.

SPRINT. The WRITE command is used for writing.

3. Close the external device/file

The external device/file assigned in the channel is released again using the EXTCLOSE

command, when the end of the program is reached (M30) or for a channel reset.

Syntax

DEF INT <Result>

DEF STRING[<n>] <Output>

…

EXTOPEN(<Result>,<ExtDev>,<SyncMode>,<AccessMode>,<WriteMode>)

…

<Output>="data output"

WRITE(<Result>,<ExtDev>,<Output>)

…

EXTCLOSE(<Result>,<ExtDev>)

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

653

Additional functions

18.9 Process DataShare - Output to an external device/file (EXTOPEN, WRITE, EXTCLOSE):

Meaning

EXTOPEN:

Pre-defined procedure to open an external device/file

<Result>:

Parameter 1: Result variable

By using the result variable value, it can be evaluated in the program as to wheth-

er the operation was successful and processing is then appropriately continued.

Type:

INT

Values:

No error

External device cannot be opened

External device is not configured

External device with invalid path configured

No access rights for external device

Usage mode: External device already "exclusively" occupied

Usage mode: External device already being "shared"

File length longer than LOCAL_DRIVE_MAX_FILESIZE

Maximum number of external devices has been exceeded

Option for LOCAL_DRIVE not set

V.24 interface has already been assigned with Easy-Message

function (only 828D)

Write mode: Data contradicts extdev.ini

Invalid external path has been programmed

External device not mounted

Job Planning

654

Programming Manual, 12/2018, A5E40869460B AB

Additional functions

18.9 Process DataShare - Output to an external device/file (EXTOPEN, WRITE, EXTCLOSE):

<ExtDev>:

Parameter 2: Symbolic identifier for the external device/file to be opened

Type:

STRING

The symbolic identifier comprises:

1. the logical device name

2. where relevant, followed by a file path (attached using "/").

The following logical device names have been defined:

"LOCAL_DRIVE":

Local CF card (pre-defined)

"CYC_DRIVE":

Reserved drive name for use in SIEMENS cycles (pre-

defined)

"/dev/ext/1", ...

Available network drives

"/dev/ext/9":

Note:

It is necessary to configure in the extdev.ini file!

"/dev/cyc/1",

Reserved drive names for use in SIEMENS cycles

"/dev/cyc/2":

Note:

It is necessary to configure in the extdev.ini file!

"/dev/v24":

V.24 interface

Note:

It is necessary to configure in the extdev.ini file!

File path:

● A file path must be specified for "LOCAL_DRIVE" and "CYC_DRIVE" e.g.

"LOCAL_DRIVE/my_dir/my_file.txt"

● The logical device names "/dev/ext/1...9" and "/dev/cyc/1...2" can be

configured:

- To already refer to a file, in which case only the logical device names may

be specified, e.g.:

"/dev/ext/4"

- Or to a directory, in which case a file path must be specified, e.g.:

"/dev/ext/5/my_dir/my_file.txt"

● It is not permissible that a file path is attached to "/dev/v24".

Note:

For the logical device names "/dev/ext/1...9", "/dev/v24" and "/dev/cyc/1...2" up-

percase/lowercase is ignored; uppercase/lowercase is significant for specifying

a path to a file. Only uppercase letters are permissible for "LOCAL_DRIVE" and

"CYC_DRIVE".

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

655

Additional functions

18.9 Process DataShare - Output to an external device/file (EXTOPEN, WRITE, EXTCLOSE):

<SyncMode>:

Parameter 3: Processing mode for the WRITE commands to this device/file

Type:

STRING

Values:

"SYN":

Synchronous writing

Program execution is stopped until the write operation

has been completed.

Successfully completing the synchronous write opera-

tion can be checked by evaluating the error variables of

the WRITE command.

"ASYN":

Asynchronous writing

Program execution is not interrupted by the WRITE

command.

Note.

In this mode, the result variable of the WRITE command

does not provide any information and always has the

value 0 (no error). In this particular mode, there is no

certainty that the WRITE command was successful.

<AccessMode>:

Parameter 4: Usage mode for this device/file

Type:

STRING

Values:

"SHARED":

Device/file is requested in the "shared" mode. Other

channels can also use the device, i.e. also open in this

mode.

"EXCL":

Device/file is exclusively used in the channel; no other

channel can use the device.

<WriteMode>:

Parameter 5: Write mode for the WRITE commands to this file/device (optional)

Type:

STRING

Values:

"APP":

Attaching

The file is always kept regarding its contents; write calls

are attached at the end.

"OVR":

Overwrite

The contents of the file are deleted and re-generated

using the subsequent write calls.

Note:

Using this parameter, the write mode configured in the extdev.ini file cannot be

overwritten. In the case of a conflict, then the EXTOPEN call is acknowledged

with error.

WRITE:

Pre-defined procedure to write output data

Job Planning

656

Programming Manual, 12/2018, A5E40869460B AB

Additional functions

18.9 Process DataShare - Output to an external device/file (EXTOPEN, WRITE, EXTCLOSE):

EXTCLOSE:

Pre-defined procedure to close an external device/file that has been opened

<Result>:

Parameter 1: Result variable

Type:

INT

Values:

No error

Invalid external path has been programmed

Error when closing the external device

<ExtDev>:

Parameter 2: Symbolic identifier for the external device/file description to be

closed, see EXTOPEN!

Note:

The identifier must be identical to the identifier specified in the EXTOPEN call!

Example

Program code

N10

DEF INT RESULT

N20

DEF BOOL EXTDEVICE

N30

DEF STRING[80] OUTPUT

N40

DEF INT PHASE

N50

EXTOPEN(RESULT,"LOCAL_DRIVE/my_file.txt","SYN","SHARED")

N60

IF RESULT > 0

N70

MSG("Error for EXTOPEN:" << RESULT)

N80

ELSE

N90

EXTDEVICE=TRUE

N100

ENDIF

…

N200

PHASE=4

N210

IF EXTDEVICE

N220

OUTPUT=SPRINT("End phase: %D",PHASE)

N230

WRITE(RESULT,"LOCAL_DRIVE/my_file.txt",OUTPUT)

N240

ENDIF

…

See also

String operations (Page 84)

Write file (WRITE) (Page 145)

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

657

Additional functions

18.10 Alarms (SETAL)

18.10

Alarms (SETAL)

Alarms can be set in an NC program. Alarms are displayed in a separate field at the user

interface. An alarm always goes hand in hand with a response from the control according to

the alarm category.

References:

For further information on alarm responses, refer to the Commissioning Manual.

Syntax

SETAL(<alarm number>[,<character string>])

Meaning

SETAL:

Keyword to program an alarm.

SETAL must be programmed in a separate NC block.

<alarm number>:

Type INT variable. Contains the alarm number.

The valid range for alarm numbers lies between 60000 and 69999, of which

60000 to 64999 are reserved for SIEMENS cycles and 65000 to 69999 are

available to users.

<character

When programming user cycle alarms, in addition, a character string with up

string>:

to four parameters can be specified.

Variable user texts can be defined in these parameters.

However, the following predefined parameters are available:

Parameter

Meaning

Channel number

Block number, label

Text index for cycle alarms

Additional alarm parameters

Note

Alarm texts must be configured in the user interface.

Note

If an alarm is to be output in the language active at the user interface, then the user requires

information about the language that is currently set at the HMI. This information can be

interrogated in the part program and in the synchronized actions using system variable

$AN_LANGUAGE_ON_HMI (see "Currently set language in the HMI (Page 916)").

Example

Program code

Comment

N100 SETAL (65000)

;Set alarm no. 65000

Job Planning

658

Programming Manual, 12/2018, A5E40869460B AB

Additional functions

18.11 Extended stop and retract (ESR)

18.11

Extended stop and retract (ESR)

The extended stop and retract function - subsequently called ESR - offers the possibility of

flexibly responding when a fault situation occurs as a function of the process:

● Extended stop

Assuming that the specific fault situation permits it, all of the axes, enabled for extended

stopping, are stopped in an orderly way.

● Retraction

The tool currently in use is retracted from the workpiece as quickly as possible.

● Generator operation (SINAMICS drive function "Vdc control")

If a parameterizable value of the DC-link voltage is fallen below, e.g. because the line

voltage fails, the electrical energy required for retraction is generated by recovering the

braking energy of the drive intended for this purpose (generator operation).

Trigger sources

General sources (NC-external/global or mode group-/channel-specific):

● Digital inputs (e.g. on NCU module or the control-internal digital output image that can be

read back ($A_IN, $A_OUT)

● Channel state ($AC_STAT)

● VDI signals ($A_DBB)

● Group messages of a number of alarms ($AC_ALARM_STAT)

Axial sources

● Emergency retraction threshold of the following axis (synchronism of electronic coupling,

$VA_EG_SYNCDIFF[<following axis>])

● Drive: DC-link warning threshold (imminent undervoltage), $AA_ESR_STAT[<axis>]

● Drive: Generator minimum speed threshold (no further regenerative rotation energy

available), $AA_ESR_STAT[<axis>].

Gating logic of the static synchronized actions: Source/response link

The static synchronized actions' flexible gating possibilities are used to trigger specific

reactions relatively quickly according to the sources.

Linking all relevant sources using static synchronized actions is the responsibility of the user.

They can selectively evaluate the source system variables as a whole or by means of bit masks,

and then make a logic operation with their desired reactions. The static synchronous actions

are effective in all operating modes.

References:

Function Manual, Synchronized Actions

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

659

Additional functions

18.11 Extended stop and retract (ESR)

Activation

Function enable

The functions generator operation, shutdown, retraction are released by setting the

corresponding control signal $AA_ESR_ENABLE. This control signal can be changed by

synchronized actions.

Function triggering

ESR is triggered jointly for all enabled axes by setting the system variable

$AC_ESR_TRIGGER.

Generator operation is "automatically" activated in the drive when an imminent DC-link

undervoltage is detected.

Drive-independent stopping and/or retraction become active when a communication failure

(between the NC and drive) is detected and when a DC-link undervoltage is detected in the

drive (configuration and enable required).

Drive-independent stopping and/or retraction can also be triggered by the NC by setting the

appropriate control signal $AN_ESR_TRIGGER (broadcast command to all drives).

References

For detailed information on ESR, see:

Function Manual, Special Functions; Extended Stop and Retract (R3)

18.11.1

NC-controlled ESR

18.11.1.1

NC-controlled retraction (POLF, POLFA, POLFMASK, POLFMLIN)

Certain initial conditions are required for NC-controlled retraction (see "NC-controlled

retraction (POLF, POLFA, POLFMASK, POLFMLIN) (Page 660)"). When these requirements

have been satisfied, then the rapid lift (LIFTFAST) configured for retraction axis(axes) in the

channel is activated by setting the system variable $AC_ESR_TRIGGER (or

$AA_ESR_TRIGGER for single axes).

Syntax

POLF(<axis>)=<position>

POLFA(<axis>,<type>,<position>)

POLFMASK(<axis_1>,<axis_2>,...)

POLFMLIN(<axis_1>,<axis_2>,...)

The following abbreviated forms are permitted for POLFA:

POLFA(<axis>,<type>) ; Abbreviated form for single axis retraction

POLFA(axis,0/1/2) ; Quick deactivation or activation

POLFA(axis,0,$AA_POLFA[axis]) ; Causes a preprocessing stop

POLFA(axis,0) ; Does not cause a preprocessing stop

Job Planning

660

Programming Manual, 12/2018, A5E40869460B AB

Additional functions

18.11 Extended stop and retract (ESR)

Meaning

POLF:

Address for specifying the target position of the retraction axis

POLF is modal.

<axis>:

Name of the geometry or channel/machine axis that retracts

<position>:

Retraction position

Type:

REAL

WCS is valid for geometry axes, otherwise MCS.

With the same identifiers for geometry and channel/machine

axes, retraction is in the WCS.

POLFA:

Predefined subprogram call for the specification of the retraction position of single

axes

<axis>:

Channel axis identifier

<type>:

Position specification mode

Type:

INT

Value:

Mark position value as invalid

Position value is absolute

Position value is incremental (distance)

Note:

If an axis is not a single axis or if the type is missing or type=0,

then a corresponding alarm is output.

<position>:

Retraction position (see above)

Note:

The position value is also accepted with type=0. Only this value

is marked as invalid and has to be reprogrammed for retraction.

POLFMASK:

Predefined subprogram call for selection of the axes that are to be retracted after

tripping of rapid lift independently of one another.

<axis_1>,…:

Names of the axes that are to be traversed to their positions

defined with POLF during rapid lift.

All the axes specified must be in the same coordinate system.

POLFMASK() without specification of an axis deactivates the rapid lift for all axes

that have been retracted independently of one another.

POLFMLIN:

Predefined subprogram call for selection of the axes that are to be retracted after

tripping of rapid lift in linear relation.

<axis_1>,…:

See above.

POLFMLIN() without specification of an axis deactivates the rapid lift for all axes

that have been retracted in linear relation.

Note

Before rapid retraction to a fixed position can be enabled via POLFMASK or POLFMLIN, a

position must have been programmed with POLF for the selected axes.

Note

If axes are enabled one after the other with POLFMASK, POLFMLIN or POLFMLIN, POLFMASK,

then the last definition always applies for the particular axis.

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

661

Additional functions

18.11 Extended stop and retract (ESR)

Note

The positions programmed with POLF and the activation by POLFMASK or POLFMLIN are

deleted when the part program is started. This means that the user must reprogram the values

for POLF and the selected axes in POLFMASK or POLFMLIN in each part program.

Note

If, when using the abbreviated form POLFA only the type is changed, then the user must ensure

that either the retraction position or the retraction path contains a practical and sensible value.

In particular, the retraction position and the retraction path have to be set again after Power

On.

Example

Retracting an individual axis:

Program code

Comment

MD37500 $MA_ESR_REACTION[AX1]=21

; NC-controlled retraction.

$AA_ESR_ENABLE[AX1]=1

POLFA(AX1,1,20.0)

; AX1 is assigned the axial retraction

position 20.0 (absolute).

$AA_ESR_TRIGGER[AX1]=1

; Retraction starts from here.

Further information

Requirements for NC-controlled retraction

● A retraction axis is configured for the NC-controlled retraction in the channel:

MD37500 $MA_ESR_REACTION = 21

● ESR must be must be enabled for this axis:

$AA_ESR_ENABLE = 1

● Delay times are defined:

MD21380 $MC_ESR_DELAY_TIME1

MD21381 $MC_ESR_DELAY_TIME2

● The axis-specific retraction positions have been configured with POLF in the part program.

● The axes are selected with POLFMASK/POLFMLIN for the NC-controlled retraction.

● The activate signals must be set for the retraction movement and remain set.

Enable and start NC-controlled reactions

If system variable $AC_ESR_TRIGGER = 1 is set and if a retraction axis is configured in this

channel (i.e. MD37500 $MA_ESR_REACTION = 21) and $AA_ESR_ENABLE = 1 is set for

this axis, then rapid lift (LIFTFAST) is activated in this channel.

The lift movement configured with POLF (or POLF) for the axes selected with POLFMASK or

POLFMLIN replaces the path motion defined for these axes in the part program.

Job Planning

662

Programming Manual, 12/2018, A5E40869460B AB

Additional functions

18.11 Extended stop and retract (ESR)

The sum of the MD21380 $MC_ESR_DELAY_TIME1 and MD21381

$MC_ESR_DELAY_TIME2 times is the maximum available for the retraction. When this time

has expired, rapid deceleration with follow-up is also initiated for the retraction axis.

Note

The extended retraction (i.e. LIFTFAST/LFPOS triggered by $AC_ESR_TRIGGER) cannot

be interrupted and can only be terminated prematurely via an emergency stop.

Note

Retraction initiated via $AC_ESR_TRIGGER is locked, in order to prevent multiple retractions.

Single axis retraction

With single axis retraction, the retraction position of the single axis must have been

programmed with POLFA and the following conditions must be satisfied:

● $AA_ESR_ENABLE = 1

● <Axis> must be a single axis at the time of triggering ($AAAA_ESR_TRIGGER = 1).

● <Type> must be either 1 or 2.

Retraction direction during rapid lift

The frame valid at the time when the lift fast is activated is taken into consideration.

Note

Frames with rotation also affect the direction of lift via POLF.

Axis replacement

Retraction axes must always be assigned to exactly one NC channel and may not be switched

among the channels. When an attempt is made to exchange a retraction axis in another

channel, an alarm is output. Only once this axis has been deactivated again using

$AA_ESR_ENABLE[AX] = 0 can it be exchanged in a new channel. Once the axis has been

exchanged, axes can be acted upon again with $AA_ESR_ENABLE[AX] = 1.

Neutral axes

Neutral axes cannot undertake NC-controlled ESR.

18.11.1.2

NC-controlled stopping

The NC-controlled stopping is activated for the stopping axes configured in the channel by

setting system variable $AC_ESR_TRIGGER (or $AA_ESR_TRIGGER for single axes).

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

663

Additional functions

18.11 Extended stop and retract (ESR)

Requirements

● A stopping axis is configured for the NC-controlled stopping in the channel:

MD37500 $MA_ESR_REACTION = 22

● ESR must be enabled for this axis:

$AA_ESR_ENABLE = 1

● Delay times are defined:

MD21380 $MC_ESR_DELAY_TIME1 (delay time, ESR axes)

MD21381 $MC_ESR_DELAY_TIME2 (ESR time for interpolatory braking)

Execution

This axis continues interpolating as programmed for the time period set in MD21380: After the

time delay specified in MD21380 has expired, controlled braking (ramp stop) is initiated: The

time period in MD21381 is the maximum available for the interpolatory controlled braking. After

this period expires, fast braking with subsequent tracking is initiated.

Example

Stopping a single axis:

Program code

Comment

MD37500 $MC_ESR_REACTION[AX1] = 22

; NC-controlled stopping.

MD21380 $MC_ESR_DELAY_TIME1[AX1] = 0.3

MD21381 $MC_ESR_DELAY_TIME2[AX1] = 0.06

$AA_ESR_ENABLE[AX1]=1

$AA_ESR_TRIGGER[AX1]=1

; Stopping starts from here.

18.11.2

Drive-integrated ESR

18.11.2.1

Configuring drive-integrated stopping (ESRS)

The drive parameters for "stopping" of the drive-integrated ESR function are configured using

the ESRS(...) function.

Syntax

ESRS(<access_1>,<stopping time_1>[,...,<axis_n>,<stopping time_n>])

Job Planning

664

Programming Manual, 12/2018, A5E40869460B AB

Additional functions

18.11 Extended stop and retract (ESR)

Meaning

ESRS(...):

Function to write to the drive parameters for the ESR function "stop-

ping"

The function:

● Must be alone in the block.

● Triggers a preprocessing stop.

● Cannot be used in synchronized actions.

<axis_1>,

Axis for which drive-integrated stopping should be configured

...,

For this axis, drive parameter p0888 (configuration) is written to in the

<axis_n>:

drive:

p0888 = 1

Type:

AXIS

Range of values:

Channel axis identifier

<stopping time_1>,

Time during which the drive continues to travel with the actual speed

...,

setpoint after a fault has occurred

<stopping time_n>:

For the specified axis, drive parameter p0892 (timer) is written to in

the drive:

p0892 = <stopping time>

Unit:

Type:

REAL

Range of values:

0.00 - 20.00

A maximum of 5 axes can be programmed in a function call; n = 5

18.11.2.2

Configuring drive-integrated retraction (ESRS)

The drive parameters for "retraction" of the drive-integrated ESR function are configured using

the ESRR(...) function.

Syntax

ESRR(<axis_1>,<retraction distance_1>,<retraction

velocity_1>[,...,<axis_n>,<retraction distance_n>,<retraction

velocity_n>])

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

665

Additional functions

18.11 Extended stop and retract (ESR)

Meaning

ESRR(...):

Function to write to the drive parameters for the ESR function "re-

tract"

The function:

● Must be alone in the block.

● Triggers a preprocessing stop.

● Cannot be used in synchronized actions.

<axis_1>,

Axis for which drive-integrated retraction should be configured

...,

For this axis, drive parameter p0888 (configuration) is written to in

<axis_n>:

the drive:

p0888 = 2

Type:

AXIS

Range of values:

Channel axis identifier

<retraction distance_1>,

For the drive, the retraction distance is converted into a retraction

...,

speed. For the specified axis, the value is written to drive parameter

<retraction distance_n>:

p0893 (speed):

p0893 = (<retraction distance _n> converted into retraction speed)

Unit:

mm/min, inch/min, degrees/min (depending

on the unit of the axis)

Type:

REAL

Range of values:

MIN - MAX

<retraction

For the drive, the retraction velocity is converted into a time. For the

velocity_1>,

specified axis, the value is written to drive parameter p0892 (timer)

...,

[s]:

<retraction

p0892 = <retraction distance_n> / <retraction velocity _n>

velocity_n>:

Unit:

mm/min, inch/min, degrees/min (depending

on the unit of the axis)

Type:

REAL

Range of values:

0.00 - MAX

A maximum of 5 axes can be programmed in a function call; n = 5

Job Planning

666

Programming Manual, 12/2018, A5E40869460B AB

Additional functions

18.12 Define blank (WORKPIECE)

18.12

Define blank (WORKPIECE)

The controller must know the shape and size of a blank to be able to display it in the graphical

simulation. The user therefore has the capability of defining blanks via the user interface or

directly in the NC program. The definitions of blanks are retained beyond a (program end/

channel/BAG) reset. They are automatically deleted the next time that the control system

powers up.

Syntax

WORKPIECE("<WP>", "<RefP>", "<ZeroOffset>", "<Type>", <Par5>,

<Par6>, ..., <Par12>)

Meaning

WORKPIECE(...):

Predefined procedure for defining a blank

Preprocessing

Yes

stop:

Alone in the

Yes

block:

Parameters:

"<WP>":

Name of the workpiece (optional)

Data type:

STRING

A specification is only necessary if there can be several workpieces

in one channel. Without specifying, "WORKP<n>" is automatically

accepted, with <n> being the number of the declaring channel.

"<RefP>":

Clamping (optional, only for milling machines)

Data type:

STRING

Range of values:

"Table"

Clamping of the fixed table

"A"

Clamping on rotary axis A

"B"

Clamping on rotary axis B

"C"

Clamping on rotary axis C

Precondition:

The table or the rotary axis must be enabled via the corresponding

machine data for the clamping of the blank (see SINUMERIK Oper-

ate Commissioning Manual).

"<ZeroOffset>":

Settable work offset for positioning the blank (not programmable)

The selection of a settable work offset for positioning the blank is

only offered for the blank entry via the user interface. For the direct

definition of the blank in the part program, the blank always relates

to the currently valid work offset.

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

667

Additional functions

18.12 Define blank (WORKPIECE)

"<Type>":

Blank shape

Data type:

STRING

Range of values:

"CYLINDER":

Cylinder

"PIPE":

Pipe

"RECTANGLE":

Centered cuboid

"BOX":

Cuboid

"N_CORNER":

Polygon with n edges

5 ... 12

<Par5> ... <Par12>:

Parameters for description of the blank shape

Data type:

REAL

The number of parameters required and their meaning depend on

the respective blank shape and the value of the bit parameter.

See:

● "Parameters for description of the blank shape" table

● "Bit parameters" table

WORPIECE():

A WORKPIECE call without parameters deletes all blank definitions.

WORPIECE(<WP>):

A WORKPIECE call with workpiece name only deletes this blank

definition.

Table 18-1

Parameters for description of the blank shape

Blank shape

Parameter

<Par5>

<Par6>

<Par7>

<Par8>

<Par9>

<Par10>

<Par11>

<Par12>

Cylinder

Bit parameter

Refer-

Length Z₁

Machin-

Outer di-

Rotation

ence point

ing dimen-

ameter d₀

about ro-

Real value that

Z₀

sion Z_B

tary axis

is interpreted as

Pipe

bit-coded inte-

Refer-

Length Z₁

Machin-

Outer di-

Wall thick-

Rotation

ger value. The

ence point

ing dimen-

ameter d₀

ness

about ro-

bits define the

Z₀

sion Z_B

(inc) / in-

tary axis

meaning of the

ner diame-

following param-

ter d₁(abs)

eters (see "Bit

Centered cuboid

Refer-

Length Z₁

Machin-

Width W

Length L

Rotation

parameters" ta-

ence point

ing dimen-

about ro-

ble).

Z₀

sion Z_B

tary axis

Cuboid

Refer-

Length Z₁

Machin-

X₀

Y₀

X₁

Y₁

ence point

ing dimen-

Z₀

sion Z_B

Polygon with n

Refer-

Length Z₁

Machin-

Number

Width

Rotation

edges

ence point

ing dimen-

of corners

across

about ro-

Z₀

sion Z_B

flats

tary axis

Job Planning

668

Programming Manual, 12/2018, A5E40869460B AB

Additional functions

18.12 Define blank (WORKPIECE)

Table 18-2

Bit parameter

Bit

Meaning

4 (0x0010)

Cuboid: X₁

= 0

inc

= 1

abs

5 (0x0020)

Cuboid: Y₁

= 0

inc

= 1

abs

6 (0x0040)

Length Z₁ (final dimension)

= 0

inc

= 1

abs

Bit 7 (0x0080)

Machining dimension Z_B

= 0

inc

= 1

abs

Bit 8 (0x0100)

Pipe: Wall thickness / inner diameter

= 0

inc

= 1

abs

9 (0x0200)

Polygon with n edges

= 0

Width across flats

= 1

Edge length

12 (0x1000)

Clamping for turning machines

= 0

Main spindle

= 1

Counterspindle

13 (0x2000)

Counterspindle

= 0

with mirroring

= 1

without mirroring

Examples

Example 1: Cylinder-shaped blank on a turning machine

=_%

Program code

Comment

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

669

Additional functions

18.12 Define blank (WORKPIECE)

Program code

Comment

WORKPIECE(,,,"CYLINDER",0,0,-200,-150,100)

; Blank definition:

; Blank shape: Cylinder

; Bit parameter=0(no bit set) →

Values for length and machining

dimension are incremental, blank

on main spindle

; Reference point(Z0)=0

; Length(Z1)=-200

; Machining dimension(ZB)=-150

; Outer diameter(d0)=100

Example 2: Pipe-shaped blank on a turning machine

=_%

Program code

Comment

WORKPIECE(,,,"PIPE",256,0,-200,-150,100,80)

; Blank definition:

; Blank shape: Pipe

; Bit parameter=256(Bit8=1) → In-

ner diameter is absolute; length

and machining dimension are in-

cremental, blank on main spindle

; Reference point(Z0)=0

; Length(Z1)=-200

; Machining dimension(ZB)=-150

; Outer diameter(d0)=100

; Inner diameter(d1)=80

Job Planning

670

Programming Manual, 12/2018, A5E40869460B AB

Additional functions

18.13 Switch language mode (G290, G291)

18.13

Switch language mode (G290, G291)

The controller gives you the capability of reading in part programs from external CNC systems

and processing them. The prerequisite is that the corresponding NC language mode (ISO

dialect) has been defined during commissioning.

Reference:

Function Manual ISO Dialects

The ISO dialect mode can be activated separately for each channel. For example, channel 1

can run in ISO dialect mode while channel 2 is active in SINUMERIK mode.

The switchover between SINUMERIK mode and ISO dialect mode is done in the NC program

via the commands of the G-group 47. The active tool, tool compensation and work offsets are

not influenced by the switchover.

Syntax

G291

G290

Meaning

G290:

Activate SINUMERIK language mode

Alone in the block:

Yes

Effective:

Modal

G291:

Activate ISO language mode

Alone in the block:

Yes

Effective:

Modal

Conditions

SINUMERIK mode

● The default of the G commands can be defined for each channel via machine data.

● No language commands from the ISO dialects can be programmed in SINUMERIK mode.

ISO dialect mode

● The ISO dialect mode can be set with machine data as the basic setting of the control

system. In ISO dialect mode, the control system then reboots by default.

● Only G commands from the ISO dialect can be programmed. The programming of

SINUMERIK G functions is not possible in ISO dialect mode.

● ISO dialect and SINUMERIK language cannot be mixed in the same NC block.

● G commands cannot be used to switch between ISO dialect M (milling) and ISO dialect T

(turning).

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

671

Additional functions

18.13 Switch language mode (G290, G291)

● Subprograms that are programmed in SINUMERIK mode can be called.

● If SINUMERIK functions are to be used, a switchover to SINUMERIK mode must first be

made (see example).

Example

Compression of linear blocks in the ISO dialect mode

Program code

Comment

N5 G290

; Activate SINUMERIK language mode.

N10 COMPON

; COMPON is a command in the Siemens lan-

guage and activates a compressor function

that replaces the successive linear

blocks with polynomial blocks with path

lengths that are as long as possible.

N15 G291

; Activate ISO language mode.

N20 G01 X100 Y100 F1000

; Since COMPON has been activated in SIN-

UMERIK mode, even linear blocks in the

ISO dialect mode can be compressed with

this function.

Job Planning

672

Programming Manual, 12/2018, A5E40869460B AB

Additional functions

18.14 Activate/deactivate load adjustment (CADAPTON, CADAPTOF)

18.14

Activate/deactivate load adjustment (CADAPTON, CADAPTOF)

Note

To use CADAPTON() and CADAPTOF(), a license is required for the following option:

● "Intelligent load adjustment" (Article number: 6FC5800-0AS11-0YB0)

Using the predefined CADAPTON() and CADAPTOF() procedures, predefined adaptation for

load-dependent adaptation of dynamic response and/or control parameters can be activated,

updated and deactivated from the part program. They are used in CYCLE782 (Page 763).

Syntax

CADAPTON(<Result>,<Axis>,<InVar>[,<InValue>])

CADAPTOF(<Result>,<Axis>,<InVar>)

Meaning

CADAPTON():

Activates adaptation relationship

CADAPTOF():

Deactivates adaptation relationship

Note:

Ignore active adaptation relationship (MD16501 = 1) CADAPTOF(), a previously pro-

grammed input value (<InVal>) remains active.

<Result>:

Result variable: Return value for the status (called by reference parameter)

Data type:

INT

Value:

No error

No valid adaptation table parameterized

<Axis> parameter invalid

<InVar> parameter invalid

Reserved

<InVal> parameter invalid

<Axis>:

Machine axis name of the input axis of the adaptation relationship

Data type:

AXIS

Range of

Machine axis names defined in the channel

values:

Note:

Using this parameter, those adaptations are addressed, which, in MD16504

$MN_CADAPT_INPUT_AX, entered a value corresponding to parameter <Axis>.

The other <InVar> and <InVal> parameters are assigned to this axis.

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

673

Additional functions

18.14 Activate/deactivate load adjustment (CADAPTON, CADAPTOF)

<InVar>:

Input variable of the adaptation relationship

Data type:

INT

Value:

The axis moment of inertia is the input variable for the adaptation

Reserved

<InVal>:

Input value of the adaptation relationship (option)

Data type:

REAL

Value:

> 0

Actual moment of inertia

= 0

Load/loading is not defined or is not known. In this particular case,

the assigned adaptations supply substitute value 1.0 as output

variable.

< 0

The call is exited with <Status> = 5 (parameter <InVal> invalid).

The last input value activated remains active.

Note:

If an input value is not programmed, the last programmed value or the default value

(= 0) after the control system has run up is active.

Example

Program code

Comment

DEF INT RESULT

; Definition of result variables

CADAPTON(RESULT,MX1,1,1.23)

; Activate adaptation with input value

IF RESULT <> 0

; Evaluate the result variables (this is

required after each CADAPTON/CADAPTOF in-

struction)

MSG("CADAPT-RESULT=" << RESULT)

STOPRE

SETAL(61000)

ENDIF

CADAPTON(RESULT,MX1,1,2.34)

; Supply adaptation with new input value

; Evaluate result variables

CADAPTOF(RESULT,MX1,1)

; Deactivate adaptation

; Evaluate result variables

Further information

Link axes

The function cannot be applied to link axes (NCU-Link function). In this case, the result variable

would supply return value 2 ("Parameter <Axis> invalid").

Job Planning

674

Programming Manual, 12/2018, A5E40869460B AB

Additional functions

18.14 Activate/deactivate load adjustment (CADAPTON, CADAPTOF)

Block search

● Block search without calculation

CADAPTON/CADAPTOF instructions that are programmed between the beginning of the

program and target block are ignored. Users must select the search target so that the

adaptations relevant for the machining section are selected.

● Block search with calculation at the contour or at block end point

The activation and/or deactivation commands - as well as possible programmed input

values - are collected, and the actual status at the end of the search is output with the

search action blocks.

● Block search with calculation in Program test (SERUPRO) mode

When SERUPRO is deactivated, the status of the adaptations achieved using the

CADAPTON/CADAPTOF instructions is transitioned into real operation.

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

675

User stock removal programs

19.1

Supporting functions for stock removal

Preprogrammed stock removal programs are provided for stock removal. Beyond this, you

have the possibility of generating your own stock removal programs using the following listed

functions:

● Generate contour table (CONTPRON)

● Generate coded contour table (CONTDCON)

● Deactivate contour preparation (EXECUTE)

● Determine point of intersection between two contour elements (INTERSEC)

(Only for tables that were generated using CONTPRON)

● Execute contour elements of a table block-by-block (EXECTAB)

(Only for tables that were generated using CONTPRON)

● Calculate circle data (CALCDAT)

Note

You can use these functions universally, not just for stock removal.

Requirements

The following must be done before calling the CONTPRON or CONTDCON functions:

● A starting point that permits collision-free machining must be approached.

● The cutting radius compensation must be deactivated with G40.

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

677

User stock removal programs

19.2 Generate contour table (CONTPRON)

19.2

Generate contour table (CONTPRON)

CONTPRON switches on the contour preparation. The NC blocks that are subsequently called

are not executed, but are split-up into individual movements and stored in the contour table.

Each contour element corresponds to one row in the two-dimensional array of the contour

table. The number of relief cuts is returned.

Syntax

Activate contour preparation:

CONTPRON(<contour table>,<machining type>,<relief cuts>,

<machining direction>)

Deactivate contour preparation and return to the normal execution mode:

EXECUTE(<ERROR>)

See "Deactivate contour preparation (EXECUTE) (Page 693)"

Meaning

CONTPRON:

Predefined procedure to activate the contour preparation to

generate a contour table

<contour table>:

Name of contour table

<machining type>:

Parameter for the machining type

Type:

CHAR

Value:

"G":

Longitudinal turning: Internal machin-

ing

"L":

Longitudinal turning: External machin-

ing

"N":

Face turning: Internal machining

"P":

Face turning: External machining

<relief cuts>:

Result variable for the number of relief cut elements that

occur

Type:

INT

<machining direction>:

Parameters for the machining direction

Type:

INT

Value:

Contour preparation, forward (default val-

ue)

Contour preparation in both directions

Example 1

Generating a contour table with:

● Name "KTAB"

● Max. 30 contour elements (circles, straight lines)

● One variable for the number of relief cut elements that occur

● One variable for error messages

Job Planning

678

Programming Manual, 12/2018, A5E40869460B AB

User stock removal programs

19.2 Generate contour table (CONTPRON)

;

NC program:

Program code

Comment

N10 DEF REAL KTAB[30,11]

; Contour table with the name KTAB and

max. 30 contour elements, parameter value

11 (number of table columns) is a fixed

quantity.

N20 DEF INT ANZHINT

; Variable for the number of relief cut

elements with the name ANZHINT.

N30 DEF INT ERROR

; Variable for error feedback signal

(0=no error, 1=error).

N40 G18

N50 CONTPRON(KTAB,"G",ANZHINT)

; Activate contour preparation.

N60 G1 X150 Z20

; N60 to N120: Contour description

N70 X110 Z30

N80 X50 RND=15

N90 Z70

N100 X40 Z85

N110 X30 Z90

N120 X0

N130 EXECUTE(ERROR)

; End filling the contour table, switch-

over to normal program mode.

N140 …

; Continue to process the table.

Contour table KTAB:

Index

Column

Line

(0)

(1)

(2)

(3)

(4)

(5)

(6)

(7)

(8)

(9)

(10)

150

82.40535663

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

679

User stock removal programs

19.2 Generate contour table (CONTPRON)

150

110

-1111

104.0362435

110

180

146.3099325

116.5650512

Explanation of the column contents:

(0)

Pointer to next contour element (to the row number of that column)

(1)

Pointer to previous contour element

(2)

Coding the contour mode for motion

Possible values for X = abc

a = 10²

G90 = 0

G91 = 1

b = 10¹

G70 = 0

G71 = 1

c = 10⁰

G0 = 0

G1 = 1

G2 = 2

G3 = 3

(3), (4)

Starting point of contour elements

(3) = abscissa, (4) = ordinate of the current plane

(5), (6)

Starting point of the contour elements

(5) = abscissa, (6) = ordinate of the current plane

(7)

Max/min indicator: Identifies local maximum and minimum values on the contour

(8)

Maximum value between contour element and abscissa (for longitudinal machin-

ing) or ordinate (for face cutting). The angle depends on the type of machining

programmed.

(9), (10)

Center point coordinates of contour element, if it is a circle block.

(9) = abscissa, (10) = ordinate

Example 2

Generating a contour table with

● Name KTAB

● Max. 92 contour elements (circles, straight lines)

● Operating mode: Longitudinal turning, external machining

● Preparation, forward and backward

Job Planning

680

Programming Manual, 12/2018, A5E40869460B AB

User stock removal programs

19.2 Generate contour table (CONTPRON)

;

NC program:

Program code

Comment

N10 DEF REAL KTAB[92,11]

; Contour table with name KTAB and max.

92 contour elements, parameter value 11

is a fixed quantity.

N20 DEF CHAR BT="L"

; Mode for CONTPRON: Longitudinal turn-

ing, external machining

N30 DEF INT HE=0

;Number of relief cut elements=0

N40 DEF INT MODE=1

; Preparation, forward and backward

N50 DEF INT ERR=0

; Error feedback signal

N100 G18 X100 Z100 F1000

N105 CONTPRON(KTAB,BT,HE,MODE)

; Activate contour preparation.

N110 G1 G90 Z20 X20

N120 X45

N130 Z0

N140 G2 Z-15 X30 K=AC(-15) I=AC(45)

N150 G1 Z-30

N160 X80

N170 Z-40

N180 EXECUTE(ERR)

; End filling the contour table, switch-

over to normal program mode.

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

681

User stock removal programs

19.2 Generate contour table (CONTPRON)

Contour table KTAB:

After contour preparation is finished, the contour is available in both directions.

Index

Column

Line

(0)

(1)

(2)

(3)

(4)

(5)

(6)

(7)

(8)

(9)

(10)

6¹⁾

7²⁾

100

0³⁾

-3

-15

-30

-1111

0⁴⁾

-30

-40

-30

1⁵⁾

2⁶⁾

0⁷⁾

-1111

0⁸⁾

-40

-30

-15

-90

-15

83⁹⁾

85¹⁰⁾

100

Explanation of column contents and comments for lines 0, 1, 6, 8, 83, 85 and 91

The explanations of the column contents given in example 1 apply.

Always in table line 0:

1) Predecessor: Line n contains the contour end (forward)

2) Successor: Line n is the contour table end (forward)

Once each within the contour elements forward:

3) Predecessor: Contour start (forward)

4) Successor: Contour end (forward)

Always in line contour table end (forward) +1:

5) Predecessor: Number of relief cuts (forward)

6) Successor: Number of relief cuts (backward)

Once each within the contour elements backward:

7) Successor: Contour end (backward)

8) Predecessor: Contour start (backward)

Always in last line of table:

9) Predecessor: Line n is the contour table start (backward)

Job Planning

682

Programming Manual, 12/2018, A5E40869460B AB

User stock removal programs

19.2 Generate contour table (CONTPRON)

10) Successor: Line n contains the contour start (backward)

Further information

Permitted traversing commands, coordinate system

The following G commands can be used for the contour programming:

● G group 1: G0, G1, G2, G3

In addition, the following are possible:

● Rounding and chamfer

● Circle programming using CIP and CT

The spline, polynomial and thread functions result in errors.

Changes to the coordinate system by activating a frame are not permissible between

CONTPRON and EXECUTE. The same applies for a change between G70 and G71 or G700 and

G710.

Replacing the geometry axes with GEOAX while preparing the contour table produces an alarm.

Relief cut elements

The contour description for the individual relief cut elements can be performed either in a

subprogram or in individual blocks.

Stock removal independent of the programmed contour direction

The contour preparation with CONTPRON was expanded so that after it has been called, the

contour table is available independent of the programmed direction.

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

683

User stock removal programs

19.3 Generate coded contour table (CONTDCON)

19.3

Generate coded contour table (CONTDCON)

With the contour preparation activated with CONTDCON, the following NC blocks that are called

are saved in a coded form in a 6-column contour table to optimize memory use. Each contour

element corresponds to one row in the contour table. When familiar with the coding rules

specified below, e.g. you can combine DIN code programs for cycles from the table lines. The

data of the output point is saved in the table line with the number 0.

Syntax

Activate contour preparation:

CONTDCON(<contour table>,<machining direction>)

Deactivate contour preparation and return to the normal execution mode:

EXECUTE(<ERROR>)

See "Deactivate contour preparation (EXECUTE) (Page 693)"

Meaning

CONTDCON:

Predefined procedure to activate the contour preparation to

generate a coded contour table

<contour table>:

Name of the contour table

<machining direction>:

Parameter for machining direction

Type:

INT

Value:

Contour preparation according to the se-

quence of contour blocks (default value)

Not permissible

Note

The G commands permitted for CONTDCON in the program section to be included in the table

are more comprehensive than for CONTPRON. Further, feedrates and feedrate type are saved

for each contour section.

Example

Generating a contour table with:

● Name "KTAB"

● Contour elements (circles, straight lines)

● Operating mode: Turning

● Machining direction: Forward

Job Planning

684

Programming Manual, 12/2018, A5E40869460B AB

User stock removal programs

19.3 Generate coded contour table (CONTDCON)

;

NC program:

Program code

Comment

N10 DEF REAL KTAB[9,6]

;Contour table with name KTAB and 9

table cells. These allow 8 contour

sets. The parameter value 6 (column

number in table) is a fixed size.

N20 DEF INT MODE = 0

; Variable for the machining direc-

tion. Standard value 0: Only in the

programmed direction of the contour.

N30 DEF INT ERROR = 0

; Variable for the error feedback sig-

nal.

N100 G18 G64 G90 G94 G710

N101 G1 Z100 X100 F1000

N105 CONTDCON (KTAB, MODE)

; Contour preparation call (MODE can

be omitted).

N110 G1 Z20 X20 F200

; Contour description.

N120 G9 X45 F300

N130 Z0 F400

N140 G2 Z-15 X30 K=AC(-15) I=AC(45)F100

N150 G64 Z-30 F600

N160 X80 F700

N170 Z-40 F800

N180 EXECUTE(ERROR)

; End filling the contour table,

switchover to normal program mode.

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

685

User stock removal programs

19.3 Generate coded contour table (CONTDCON)

Contour table KTAB:

Column index

Line index

Contour

End point

Center point

Feedrate

mode

abscissa

ordinate

abscissa

ordinate

100

11031

200

111031

300

11031

400

11032

-15

100

11031

-30

600

11031

-30

700

11031

-40

800

Explanation of the column contents:

Line 0 Coding for the starting point:

Column 0:

10⁰ (ones digit): G0 = 0

10¹ (tens digit): G70 = 0, G71 = 1, G700 = 2, G710 = 3

Column 1:

Starting point abscissa

Column 2:

Starting point ordinate

Column 3-4:

Column 5:

Line index of last contour piece in the table

Lines 1-n: Entries for contour pieces

Column 0:

10⁰ (ones digit): G0 = 0, G1 = 1, G2 = 2, G3 = 3

10¹ (tens digit): G70 = 0, G71 = 1, G700 = 2, G710 = 3

10² (hundreds digit): G90 = 0, G91 = 1

10³ (thousands digit): G93 = 0, G94 = 1, G95 = 2, G96 = 3

10⁴ (ten thousands digit): G60 = 0, G44 = 1, G641 = 2, G642 = 3

10⁵ (hundred thousands digit): G9 = 1

Column 1:

End point abscissa

Column 2:

End point ordinate

Column 3:

Center point abscissa for circular interpolation

Column 4:

Center point ordinate for circular interpolation

Column 5:

Feedrate

Job Planning

686

Programming Manual, 12/2018, A5E40869460B AB

User stock removal programs

19.3 Generate coded contour table (CONTDCON)

Further information

Permitted traversing commands, coordinate system

The following G groups and G commands can be used for the contour programming:

G group 1:

G0, G1, G2, G3

G group 10:

G60, G64, G641, G642

G group 11:

G group 13:

G70, G71, G700, G710

G group 14:

G90, G91

G group 15:

G93, G94, G95, G96, G961

In addition, the following are possible:

● Rounding and chamfer

● Circle programming using CIP and CT

The spline, polynomial and thread functions result in errors.

Changes to the coordinate system by activating a frame are not permissible between

CONTDCON and EXECUTE. The same applies for a change between G70 and G71 or G700 and

G710.

Replacing the geometry axes with GEOAX while preparing the contour table produces an alarm.

Machining direction

The contour table generated using CONTDCON is used for stock removal in the programmed

direction of the contour.

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

687

User stock removal programs

19.4 Determine point of intersection between two contour elements (INTERSEC)

19.4

Determine point of intersection between two contour elements

(INTERSEC)

INTERSEC determines the point of intersection of two normalized contour elements from the

contour tables generated using CONTPRON.

Syntax

<Status>=INTERSEC(<contour table_1>[<contour element_1>],

<contour table_2>[<contour element_2>],<intersection

point>,<machining type>)

Meaning

INTERSEC:

Predefined function to determine the point of intersection between

two contour elements from the contour tables generated with

CONTPRON

<Status>:

Variable for the point of intersection status

Type:

BOOL

Value:

TRUE

Point of intersection found

FALSE

No intersection found

<contour table_1>:

Name of the first contour table

<contour element_1>:

Number of the contour element of the first contour table

<contour table_2>:

Names of the second contour table

<contour element_2>:

Number of the contour element of the second contour table

<point of intersection>:

Intersection coordinates in the active plane (G17 / G18 / G19)

Type:

REAL

<machining type>:

Parameter for the machining type

Type:

INT

Value:

Point of intersection calculation in the active

plane with parameter 2

(standard value)

Point of intersection calculation independent of

the transferred plane

Note

Please note that the variables must be defined before they are used.

The values defined with CONTPRON must be observed when transferring the contours:

Parameter

Meaning

Coding of contour mode for the movement

Contour start point abscissa

Contour start point ordinate

Contour end point abscissa

Contour end point ordinate

Job Planning

688

Programming Manual, 12/2018, A5E40869460B AB

User stock removal programs

19.4 Determine point of intersection between two contour elements (INTERSEC)

Parameter

Meaning

Center point coordinates for abscissa (only for circle contour)

Center point coordinates for ordinate (only for circle contour)

Example

Calculate the intersection of contour element 3 in table TABNAME1 and contour element 7 in

table TABNAME2. The intersection coordinates in the active plane are stored in the variables

ISCOORD (1st element = abscissa, 2nd element = ordinate). If no intersection exists, the

program jumps to NOCUT (no intersection found).

Program code

Comment

DEF REAL TABNAME1[12,11]

; Contour table 1

DEF REAL TABNAME2[10,11]

; Contour table 2

DEF REAL ISCOORD [2]

; Variable for the intersection coor-

dinates.

DEF BOOL ISPOINT

; Variable for the intersection sta-

tus.

DEF INT MODE

; Variable for the machining type.

…

MODE=1

; Calculation independent of the ac-

tive plane.

N10 ISPOINT=INTERSEC(TABNAME1[3],TABNAME2[7],

; Intersection of the contour ele-

ISCOORD,MODE)

ments call.

N20 IF ISPOINT==FALSE GOTOF NOCUT

; Jump to NOCUT.

…

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

689

User stock removal programs

19.5 Execute the contour elements of a table block-by-block (EXECTAB)

19.5

Execute the contour elements of a table block-by-block (EXECTAB)

Using EXECTAB, you can execute the contour elements of a table - that were generated, e.g.

with CONTPRON - block-by-block.

Syntax

EXECTAB(<contour table>[<contour element>])

Meaning

EXECTAB:

Predefined procedure to execute a contour element

<contour table>:

Name of the contour table

<contour element>:

Number of the contour element

Example

Contour elements 0 to 2 in table KTAB should be executed block-by-block.

Program code

Comment

N10 EXECTAB(KTAB[0])

; Traverse element 0 of table KTAB.

N20 EXECTAB(KTAB[1])

; Traverse element 1 of table KTAB.

N30 EXECTAB(KTAB[2])

; Traverse element 2 of table KTAB.

Job Planning

690

Programming Manual, 12/2018, A5E40869460B AB

User stock removal programs

19.6 Calculate circle data (CALCDAT)

19.6

Calculate circle data (CALCDAT)

With CALCDAT, you can calculate the radius and the circle center point coordinates from the

three or four points known along the circle. The specified points must be different.

Where four points do not lie directly on the circle an average value is formed for the circle

center point and the radius.

Note

Calculation regulation for the averaging

The arc calculation is performed four times:

1. With circle points 1, 2, 3

2. With circle points 1, 2, 4

3. With circle points 1, 3, 4

4. With circle points 2, 3, 4

The values of the circle center point coordinates abscissa and ordinate are calculated by

adding the abscissa and ordinate values of the four arc calculations and dividing by four.

The radius is calculated by forming the root from the sum of the four radii from the arc

calculations and multiplying the result with 0.5.

Syntax

<Status>=CALCDAT(<circle points>[<number>,<type>],<number>,<result>)

Meaning

CALCDAT:

Predefined function to calculate the radius and center point coordinates

of a circle from three or four points

<Status>:

Variable for the circle calculation status

Type:

BOOL

Value:

TRUE

The specified points lie on a circle.

FALSE

The specified points do not lie on a circle.

<circle points>[]:

Variable to specify the circle points

using parameters

<number>:

Number of circle points (3 or 4)

<type>:

Type of coordinate data,

e.g. 2 for 2-point coordinates

<number>:

Parameter for the number of the points used for the calculation (3 or 4)

<result>[3]:

Variable for result:

Circle center point coordinates and radius

Circle center point coordinate: Abscissa value

Circle center point coordinate: Ordinate value

Radius

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

691

User stock removal programs

19.6 Calculate circle data (CALCDAT)

Note

Please note that the variables must be defined before they are used.

Example

Using three points it should be determined as to whether they are located on a circle segment.

(5* > @

;

(5* > @

Program code

Comment

N10 DEF REAL PT[3,2]=(20,50,50,40,65,20)

; Variable to specify the points

of a circle.

N20 DEF REAL RES[3]

; Variable for result.

N30 DEF BOOL STATUS

; Variable for status.

N40 STATUS=CALCDAT(PKT,3,ERG)

; Call of the determined circle

data.

N50 IF STATUS == FALSE GOTOF ERROR

; Jump to error.

Job Planning

692

Programming Manual, 12/2018, A5E40869460B AB

User stock removal programs

19.7 Deactivate contour preparation (EXECUTE)

19.7

Deactivate contour preparation (EXECUTE)

EXECUTE deactivates the contour preparation and at the same time the system returns to the

normal execution mode.

Syntax

EXECUTE(<ERROR>)

Meaning

EXECUTE:

Predefined procedure to terminate contour preparation

<ERROR>:

Variable for the error feedback signal

Type:

INT

The value of the variable indicates whether the contour was able to be prepared error-

free:

Error

No error

Example

Program code

N30 CONTPRON(...)

N40 G1 X... Z

N100 EXECUTE(...)

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

693

Programming cycles externally

20.1

Technology cycles

20.1.1

Introduction

Contents

This section contains a description of the cycles for the turning, milling, and grinding

technologies.

Structure

The description of a cycle is structured as follows:

● Syntax

Cycle name and call sequence of the transfer parameters

● Parameters

Tables to explain the individual parameters

Parameter description

The following data is specified in the table for a parameter: Name, description, value range,

and dependencies on other parameters.

The column for reference to the parameter in the screen form is provided to more easily locate

values programmed on the control when externally generated cycle calls are recompiled.

"For interface only" parameters

Certain parameters are marked "for interface only" in the table. These are not relevant to

operation of the cycle. They are only needed in order to be able to recompile cycle calls

completely. If they are not programmed the cycle can still be recompiled; the fields are then

identified by color and must be completed in the mask.

"Reserved" parameters

Parameters that are described as "reserved" must be programmed with the value 0 or a comma

so that the assignment of the following call parameters matches the internal cycle parameters.

Exception: string parameters with the value "" or a comma.

Repeating cycles on a position pattern

Drilling and milling cycles can be repeated on the position pattern (modal calls). In such cases

MCALL should be written in the same line before the cycle, e.g. MCALL CYCLE83(...).

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

695

SINUMERIK 840D sl/828D. Job Planning. Programming Manual (2010-2018) - page 10