SINUMERIK 840D sl. Service - Functions. Manual (2018-2020)

Punching and nibbling

12.3 Activation and deactivation

The delay time for stroke initiation can be adjusted in machine data:

MD26018 $MC_NIBBLE_PRE_START_TIME

Example:

With an IPO cycle of 5 ms, a stroke shall be released two cycles after reaching the interpolation

end:

⇒ MD26018 $MC_NIBBLE_PRE_START_TIME = 0.01 [s]

A pre-initiation time can also be programmed in setting data:

SD42402 $SC_NIBPUNCH_PRE_START_TIME

This setting takes effective only if MD26018 = 0 has been set.

Monitoring of the input signal

If the "stroke active" signal is fluctuating between strokes due to plunger overshoots, for

example, the message "undefined punching signal" can be also be output when interpolation is

stopped.

The message output is dependent on the setting in machine data:

MD26020 $MC_NIBBLE_SIGNAL_CHECK

MD26020 = 0

No alarm

MD26020 = 1

Alarm

Minimum period between two strokes

A minimum time interval between two consecutive strokes can be programmed in setting data:

SD42404 $SC_MINTIME_BETWEEN_STROKES

Example:

There must be a minimum delay of at least 1.3 seconds between two stroke initiations

irrespective of physical distance:

⇒ SD42404 $SC_MINTIME_BETWEEN_STROKES = 1.3 [s]

If a punching dwell time (PDELAYON) is also programmed, then the two times are applied

additively.

If a pre-initiation time at G603 is programmed, it will be effective only if the end of interpolation

is reached before the time set in SD42404.

The programmed time becomes operative immediately. Depending on the size of the block

buffer, strokes that have already been programmed can be executed with this minimum interval.

The following programming measures (example) can be taken to prevent this:

Program code

N...

N100 STOPRE

N110 $SC_ MINTIME_BETWEEN_STROKES = 1.3

Technologies

Function Manual, 10/2020, 6FC5397-8GP40-0BA1

253

Punching and nibbling

12.3 Activation and deactivation

The function is not active when SD42404 = 0.

Path-dependent acceleration

An acceleration characteristic can be defined using the PUNCHACC (Smin, Amin, Smax,

Amax) language command. This command can be used to define different acceleration rates

depending on the distance between holes.

Example 1:

381&+$&&

6 >PP@

The characteristic defines the following acceleration rates:

Distance be-

Acceleration

tween holes

< 2 mm

The axis accelerates at a rate corresponding to 50% of maximum acceleration.

2 - 10 mm

Acceleration is increased to 100%, proportional to the spacing.

> 10 mm

The axis accelerates at the maximum rate (100%).

Example 2:

381&+$&&

6 >PP@

Technologies

254

Function Manual, 10/2020, 6FC5397-8GP40-0BA1

Punching and nibbling

12.3 Activation and deactivation

The characteristic defines the following acceleration rates:

Distance be-

Acceleration

tween holes

< 3 mm

The axis accelerates at a rate corresponding to 75% of maximum acceleration.

3 - 8 mm

Acceleration is reduced to 25%, proportional to the spacing.

> 10 mm

The axis accelerates at a rate of 25%.

If a reduced acceleration rate has already been programmed via ACC, then the acceleration

limits defined with PUNCHACC refer to the reduced acceleration rate.

The function is deselected with:

S_min = S_max = 0

The acceleration rate programmed beforehand with ACC remains operative.

Block search

In the case of a search for a block containing a nibbling function, it is possible to program

whether the punch stroke is executed at the block beginning or suppressed.

The setting is programmed in machine data:

MD11450 $MN_SEARCH_RUN_MODE

Bit

Value

Meaning

Punch stroke at beginning of block is suppressed.

Punch stroke at beginning of block is executed.

Further information:

Function Manual Basic Functions; Mode Group, Channel, Program Operation, Reset Response,

Block Search

12.3.3

Compatibility with earlier systems

Use of M functions

As in earlier versions, macro technology allows special M functions to be used instead of

language commands (compatibility).

The M functions and equivalent language commands as used in earlier systems are as follows:

M20, M23

≙ SPOF

M22

≙ SON

M25

≙ PON

M26

≙ PDELAYON

Technologies

Function Manual, 10/2020, 6FC5397-8GP40-0BA1

255

Punching and nibbling

12.3 Activation and deactivation

Note

M functions can be configured in machine data.

When M functions are assigned to language commands, it must be noted that M functions are

organized in auxiliary function groups.

Examples

DEFINE M20 AS SPOF

Punching/nibbling OFF

DEFINE M20 AS SPOF M=20

Punching with auxiliary function output

DEFINE M20 AS SPOF PDELAYOF Punching/nibbling OFF and punching with delay OFF

DEFINE M22 AS SON

Nibbling ON

DEFINE M22 AS SON M=22

Nibbling ON with auxiliary function output

DEFINE M25 AS PON

Punching ON

DEFINE M25 AS PON M=25

Punching ON with auxiliary function output

DEFINE M26 AS PDELAYON

Punching with delay ON

DEFINE M26 AS PDELAYON M=26 Punching and auxiliary function output

Programming example:

Program code

Comment

N100 X100 M20

; position without punch initiation

N110 X120 M22

; Activate nibbling, before and after motion

; stroke initiation

N120 X150 Y150 M25

; Activate punching, initiate stroke at end

; of the motion

Technologies

256

Function Manual, 10/2020, 6FC5397-8GP40-0BA1

Punching and nibbling

12.4 Automatic path segmentation

12.4

Automatic path segmentation

12.4.1

General information

Function

One of the following two methods can be applied to automatically segment a programmed

traversing path:

• Path segmentation with maximum path segment programmed via language command SPP

• Path segmentation with a number of segments programmed via language command SPN

Both functions generate sub-blocks independently.

In earlier systems

• SPP<number> corresponds to E<number>

• SPN<number> corresponds to H<number>

Since addresses E and H now represent auxiliary functions, language commands SPP and SPN

are used to avoid conflicts. The new procedure is therefore not compatible with those

implemented in earlier systems. Both language commands (SPP and SPN) can be configured.

Note

The values programmed with SPP are either mm or inch settings depending on the initial setting

(analogous to axes).

The automatic path segmentation function ensures that the path is divided into equidistant

sections with linear and circle interpolation.

When the program is interrupted and automatic path segmentation is active (SPP/SPN), the

contour can be reentered only at the beginning of the segmented block. The first punch stroke

is executed at the end of this sub-block.

SPP and SPN can be activated only if geometry axes are configured.

SPP

The automatic path segmentation function SPP divides the programmed traversing path into

sections of equal size according to the segment specification.

The following conditions apply:

• Path segmentation is active only when SON or PON is active.

(Exception: MD26014 $MC_PUNCH_PATH_SPLITTING = 1)

• SPP is modally active, i.e. the programmed segment remains valid until it is programmed

again, but it can be suppressed on a block-by-block (non-modal) basis by means of SPN.

• The path segments are rounded off by the control system if required so that a total

programmed distance can be divided into an integral number of path sections.

• The path segment unit is either mm/stroke or inch/stroke (depending on axis settings).

Technologies

Function Manual, 10/2020, 6FC5397-8GP40-0BA1

257

Punching and nibbling

12.4 Automatic path segmentation

• If the programmed SPP value is greater than the traversing distance, then the axis is

positioned on the programmed end position without path segmentation.

• SPP = 0, reset or program end delete the programmed SPP value. The SPP value is not

deleted when punching/nibbling is deactivated.

SPN

The automatic path segmentation function SPN divides the traversing path into the

programmed number of path segments.

The following conditions apply:

• Path segmentation is active only when SON or PON is active.

(Exception: MD26014 $MC_PUNCH_PATH_SPLITTING = 1)

• SPN has a non-modal action.

• Any previously programmed SPP value is suppressed for the block containing SPN, but is re-

activated again in the following blocks.

Supplementary conditions

• The path segmentation function is operative with linear and circular interpolation.

The interpolation mode remains unchanged, i.e. circles are traversed when circular

interpolation is selected.

• If a block contains both SPN (number of strokes) and SPP (stroke path), then the number of

blocks is activated in the current block while the stroke path is activated in all blocks that

follow.

• Path segmentation is active only in conjunction with punching or nibbling functions.

(Exception: MD26014 $MC_PUNCH_PATH_SPLITTING = 1).

• Any programmed auxiliary functions are output before, during the first or after the last sub-

block.

• In the case of blocks without traversing information, the rules which govern the

programming of SON and PON also apply to SPP and SPN. In other words, a stroke is initiated

only if an axis motion has been programmed.

12.4.2

Operating characteristics with path axes

MD26010

All axes defined and programmed via machine data:

MD26010 $MC_PUNCHNIB_AXIS_MASK

are traversed along path sections of identical size with SPP and SPN until the programmed end

point is reached. This also applies to rotatable tool axes if programmed. The response can be

adjusted for single axes.

Technologies

258

Function Manual, 10/2020, 6FC5397-8GP40-0BA1

Punching and nibbling

12.4 Automatic path segmentation

Example of SPP

Program code

Comment

N1 G01 X0 Y0 SPOF

; positioning without punch initiation

N2 X75 SPP=25 SON

; nibbling with feedrate value 25 mm; initiate punch

; before the first movement and after each

; path segment.

N3 Y10

; positioning with reduced SPP value, because

; traversing distance < SPP value, and initiate punch

; after the movement.

N4 X0

Reposition with punch initiation

after each path section.

633

If the programmed path segmentation is not an integral multiple of the total path, then the feed

path is reduced.

Technologies

Function Manual, 10/2020, 6FC5397-8GP40-0BA1

259

Punching and nibbling

12.4 Automatic path segmentation

633ಿ

633

;

[

X2/Y2:

Programmed traversing distance

SPP:

Programmed SPP value

SPP':

Automatically rounded-off offset distance

Figure 12-4

Path segmentation

Example of SPN

The number of path segments per block is programmed via SPN.

A value programmed via SPN takes effect on a non-modal basis for both punching and nibbling

applications. The only difference between the two modes is with respect to the first stroke. This

is normally executed at the beginning of the first segment with nibbling operations and at its end

with punching operations. This means that when n segments are programmed, n strokes are

executed with punching operations but n+1 with nibbling. Furthermore, where no travel

information is available, only a single stroke is executed, even if several are programmed. Should

it be necessary to generate several strokes at one position, then the corresponding number of

blocks without traversing information must be programmed.

Program code

Comment

N1 G01 X0 Y0 SPOF

; positioning without punch initiation

N2 X75 SPN=3 SON

; activate nibbling. The total path is

; divided into 3 path segments. Before the first

; movement and at the end of each path segment, a

; stroke is initiated.

Technologies

260

Function Manual, 10/2020, 6FC5397-8GP40-0BA1

Punching and nibbling

12.4 Automatic path segmentation

Example

;

Figure 12-5

Workpiece

Extract from program

Program code

Comment

N100 G90 X130 Y75 F60 SPOF

; positioning to starting point (1) of the

; vertical nibbling path segments

N110 G91 Y125 SPP=4 SON

; end point coordinates (incremental)

; path segment: 4 mm, activate nibbling

N120 G90 Y250 SPOF

; absolute dimensioning, positioning at

; the start point (2) of the horizontal

; nibbling path segment

N130 X365 SPN=4 SON

; end point coordinates, 4 path segments,

; activate nibbling

N140 X525 SPOF

; positioning to starting point (3) of the

; inclined nibbling path

N150 X210 Y75 SPP=3 SON

; end point coordinates, path segment: 3

mm,

; activate nibbling

N160 X525 SPOF

; positioning to starting point (4) of the

; nibbling path on pitch circle path

N170 G02 G91 X-62.5 Y62.5 I0 J62.5 SON

; incremental circular interpolation with

; activate parameters,

Technologies

262

Function Manual, 10/2020, 6FC5397-8GP40-0BA1

Punching and nibbling

12.4 Automatic path segmentation

Program code

Comment

; nibbling

N180 G00 G90 Y300 SPOF

; positioning

12.4.3

Response in connection with single axes

MD26016

The path of single axes programmed in addition to path axes is distributed evenly among the

generated intermediate blocks as standard.

In the following example, the additional rotary axis C is defined as a synchronous axis.

If this axis is programmed additionally as a "Punch-nibble axis":

MD26010 $MC_PUNCHNIB_AXIS_MASK = 1,

, then the behavior of the synchronous axis can be varied as a function of machine data:

MD26016 $MC_PUNCH_PARTITION_TYPE

Programming example:

Program code

N10 G90 G1 PON X10 Y10 C0 F10000

N20 SPP=5 X25 C45

N30 G3 SPN=3 X35 Y20 I0 J10 C90

MD26016 $MC_PUNCH_PARTITION_TYPE=0 (default setting)

With this setting, the axes behave as standard, i.e. the programmed special axis motions are

distributed among the generated intermediate blocks of the active path segmentation function

in all interpolation modes.

In block N20, the C axis is rotated through 15° in each of the three intermediate blocks. The axis

response is the same in block N30, in the case of circular interpolation (three sub-blocks, each

with 15° axis rotation).

Technologies

Function Manual, 10/2020, 6FC5397-8GP40-0BA1

263

Punching and nibbling

12.4 Automatic path segmentation

& r

[

MD26016 $MC_PUNCH_PARTITION_TYPE=1

In contrast to the behavior described above, here the synchronous axis travels the entire

programmed rotation path in the first sub-block of the selected path segmentation function.

Applied to the example, the C axis already reaches the programmed end position C=45 when it

reaches X position X=15. It behaves in the same way in the circular interpolation block below.

& r

[

Technologies

264

Function Manual, 10/2020, 6FC5397-8GP40-0BA1

Punching and nibbling

12.4 Automatic path segmentation

MD26016 $MC_PUNCH_PARTITION_TYPE=2

MD26016=2 is set in cases where the axis must behave as described above in linear interpolation

mode, but according to the default setting in circular interpolation mode (see 1st case).

The axis behavior for the example is then as follows: In block N20, the C axis is rotated to C=45°

in the first sub-block. The following circular interpolation block rotates the C axis through 15° in

every sub-block.

& r

[

The axis response illustrated in the diagram above can be particularly useful when applied to the

axis of a rotatable tool in cases where it is used to place the tool in a defined direction (e.g.

tangential) in relation to the contour, but where the tangential control function must not be

applied. However, it is not a substitute for the tangential control function since the start and end

positions of the rotary axis must always be programmed.

Note

Additional offset motions of special axes (in this case, rotary axis C) are implemented via a zero

offset.

Technologies

Function Manual, 10/2020, 6FC5397-8GP40-0BA1

265

Punching and nibbling

12.4 Automatic path segmentation

Supplementary conditions

• If the C axis is not defined as a "Punch-nibble axis", then the C axis motion path is not

segmented in block N30 in the above example nor is a stroke initiated at the block end.

• If the functionality described above is to be implemented in a variant not specific to nibbling

applications, but with alignment of the special axis, then stroke initiation can be suppressed

by the following PLC interface signal:

DB 21, 22 DBX3.2 (stroke suppression)

(Application: e.g. alignment of electron beam during welding)

A similar response can be programmed with the following machine data setting:

MD26014 $MC_PUNCH_PATH_SPLITTING=1

In this case, the path is segmented irrespective of punching or nibbling functions.

Technologies

266

Function Manual, 10/2020, 6FC5397-8GP40-0BA1

Punching and nibbling

12.5 Rotatable tool

12.5.2

Coupled motion of punch and die

Function

Using the standard function "Coupled motion", it is possible to assign the axis of the die as a

coupled motion axis to the rotary axis of the punch.

Activation

The "Coupled motion" function is activated or deactivated with language commands TRAILON

and TRAILOF respectively.

Further information

Function Manual Axes and Spindles; Axis Couplings

Example

Example of a typical nibbling machine with rotatable punches where C is the punch axis and C1

the die axis:

Program code

Comment

TRAILON (C1, C, 1)

;Enabling the coupled-motion grouping

G01 X100 Y100 C0 PON

;Initiate stroke with C axis /

;C1 axis position C=0=C1

X150 C45

;Initiate stroke with C axis /

;C1 axis position C=45=C1

M30

Basic position

No coupled-motion groupings are active after power up. Once the two tool axes have

approached the reference point, the coupled-motion grouping is not generally separated again.

This can be achieved by:

• Program single activation of the coupled-motion grouping (see example above)

• Program MD setting:

MD20110 $MC_RESET_MODE_MASK, bit 8=1

In this way, the coupled-motion grouping remains active after RESET/part program start or end.

Technologies

268

Function Manual, 10/2020, 6FC5397-8GP40-0BA1

Punching and nibbling

12.5 Rotatable tool

12.5.3

Tangential control

Function

The "tangential control" function aligns the rotary axis used for positioning the punching/

nibbling tool so that it is tangential to the programmed path. In connection with tangential

control, this axis is called the tangential axis. The linear axes of the machining plane are the

leading axes of the tangential coupling. The tangential axis is the following axis that is aligned

to the path tangent of the lead axes. An additive offset angle for the tangent angle can also be

programmed for the tangential axis.

If the punching/nibbling tool (die and die plate) is moved via two separate rotary axes, the

second rotary axes can be coupled to the tangential axis via "coupled motion".

Note

Switch-on sequence

In the NC program, the tangential control must first be defined and then the coupled motion

must be activated.

Further information

A detailed description of the tangential control can be found in the Axis and Spindles Function

Manual.

Example: Linear interpolation

Assumptions

• The punching/nibbling tool is subdivided into bottom and top tool

• The bottom tool and top tool are moved by different rotary axes (C/C1).

• The linear axes X and Y are the leading axes (machining plane G17)

Program code

Comment

N2 TANG (C, X, Y, 1, "B")

; definition tangential control

; leading axes: X, Y

; following axis: C

; coupling factor: 1

; basic coordinate system

N5 G0 X10 Y5

; starting position

N8 TRAILON (C1, C, 1)

; coupled motion ON

N10 Y10 C225 PON F60

; C/C1 axis → 225°

; nibbling initiation ON, → stroke

N15 X20 Y20 C45

; C/C1 axis → 45° → stroke

N20 X50 Y20 C90 SPOF

; C/C1 axis → 90°

; stroke initiation: OFF

Technologies

Function Manual, 10/2020, 6FC5397-8GP40-0BA1

269

Punching and nibbling

12.5 Rotatable tool

Program code

Comment

N25 X80 Y20 SPP=10 SON

; path segmentation: ON

; path segment: 10 mm → 4 lifts

; punch initiation: ON

N30 X60 Y40 SPOF

; positioning

; stroke initiation: OFF

N32 TANGON (C, 180)

; tangential control: ON

; offset angle: 180°

N35 X30 Y70 SPN=3 PON

; path segmentation: 3 path segments → lift

; nibbling initiation: ON

N40 G91 C45 X-10 Y-10

; C/C1: 90° (-135°+180°+45°) → lift

N42 TANGON (C, 0)

; tangential control: ON

; offset angle: 0°

N45 G90 Y30 SPN=3 SON

; path segmentation → 3 lifts

; punch initiation: ON

N50 SPOF TANGOF

; stroke initiation: OFF

; tangential control: OFF

N55 TRAILOF (C1, C)

; coupled motion: OFF

N60 M2

[

① Mounting position 0°

② Positioning

③ Stroke

Technologies

270

Function Manual, 10/2020, 6FC5397-8GP40-0BA1

Punching and nibbling

12.5 Rotatable tool

Example: Circular interpolation

In circular interpolation mode, particularly when path segmentation is active, the tool axes

rotate along a path tangentially aligned to the programmed path axes in each sub-block.

Program code

Comment

N2 TANG (C, X, Y, 1, "B")

;

definition tangential control

;

leading axes: X, Y

;

following axis: C

;

coupling factor: 1

;

basic coordinate system

N5 G0 F60 X10 Y10

;

starting position

N8 TRAILON (C1, C, 1)

;

coupled motion: ON

N9 TANGON (C, -90)

;

tangential control: ON

;

offset angle: -90° or 270°

N10

G02 X30 Y30 I20 J0 SPN=2 PON

;

circular interpolation

;

path segmentation → 2 lifts

N15

G0 X70 Y10 SPOF

;

positioning

;

stroke initiation: OFF

N17

TANGON (C, 90)

;

tangential control: ON

;

offset angle: 90°

N20

G03 X35,86 Y24,14 CR=20 SPP=16 SON

;

circular interpolation

;

path segmentation → 4 lifts

;

punch initiation: ON

N25

G0 X74,14 Y35,86 C0 PON

;

positioning

;

C/C1 axis: 0°

;

nibbling initiation: ON

N27

TANGON (C, 0)

;

tangential control: ON

;

offset angle: 0°

N30

G03 X40 Y50 I-14,14 J14,14 SPN=5 SON

;

circular interpolation

;

path segmentation → 5 lifts

;

punch initiation: ON

N35

G0 X30 Y65 C90 SPOF

;

positioning

;

stroke initiation: OFF

N40

G91 X-10 Y-25 C180

;

positioning, incremental

;

C/C1 axis: +180°

;

⇒ 270° absolute

N43

TANGOF

;

tangential control: OFF

N45

G90 G02 Y60 I0 J10 SPP=2 PON

;

circular interpolation

;

path segmentation → 2 lifts

N50

SPOF

;

stroke initiation: OFF

N55

TRAILOF (C1, C)

;

coupled motion: OFF

N60

Technologies

Function Manual, 10/2020, 6FC5397-8GP40-0BA1

271

Punching and nibbling

12.7 Supplementary conditions

[

① Mounting position 0°

② Positioning

③ Stroke

12.6

Protection zones

Clamping protection zone

The "clamping protection zone" function is contained as a subset in the "Protection zones"

function. Its purpose is to simply monitor whether clamps and tool could represent a mutual risk.

Note

No by-pass strategies are implemented for cases where the clamp protection is violated.

Further information

Function Manual Monitoring and Compensating; Axis Monitoring, Protection Zones

12.7

Supplementary conditions

Availability of function "Punching and nibbling"

The function is an option ("Punching and nibbling functions"), which must be assigned to the

hardware through the license management.

Technologies

272

Function Manual, 10/2020, 6FC5397-8GP40-0BA1

Punching and nibbling

12.8 Examples

12.8

Examples

12.8.1

Examples of defined start of nibbling operation

Example 1

Example of defined start of nibbling operation

Program code

Comment

N10 G0 X20 Y120 SPP= 20

; Position 1 is approached

N20 X120 SON

; Defined start of nibbling, first stroke at

; "1", last stroke at "2"

N30 Y20

; Defined start of nibbling, first stroke at

; "3", last stroke at "4"

N40 X20

; Defined start of nibbling, first stroke at

; "5", last stroke at "6"

N50 SPOF

N60 M2

[

Technologies

Function Manual, 10/2020, 6FC5397-8GP40-0BA1

273

Punching and nibbling

12.8 Examples

Example 2

This example utilizes the "Tangential control" function. Z has been selected as the name of the

tangential axis.

Program code

Comment

N5 TANG (Z, X, Y, 1, "B")

; Define tangential axis

N8 TANGON (Z, 0)

; Select tangential control

N10 G0 X20 Y120

; Position 1 is approached

N20 X120 SPP=20 SON

; Defined start of nibbling,

; tangential control selected,

; first stroke at "1", last stroke at "2"

N30 SPOF TANGOF

; Deselect nibbling mode and deselect

; tangential control

N38 TANGON (Z, 90)

; Select tangential control

N40 Y20 SON

; Defined start of nibbling,

; tangential control selected,

; first stroke at "2" rotated 90 degrees to

; block N20, last stroke at "3"

N50 SPOF TANGOF

; Deselect nibbling mode and deselect

; tangential control

N60 M2

[

Technologies

274

Function Manual, 10/2020, 6FC5397-8GP40-0BA1

Punching and nibbling

12.8 Examples

Examples 3 and 4 for defined start of nibbling

Example 3: Programming of SPP

Program code

Comment

N5 G0 X10 Y10

; Positioning

N10 X90 SPP=20 SON

; Defined start of nibbling,

; 5 punches initiated

N20 X10 Y30 SPP=0

; One punch is initiated at the end of the path

N30 X90 SPP=20

; 4 punches initiated at intervals of 20 mm

N40 SPOF

N50 M2

Example 4 Programming of SPN

Program code

Comment

N5 G0 X10 Y10

; Positioning

N10 X90 SPN=4 SON

; Defined start of nibbling, 5

; 5 punches initiated

N20 X10 Y30 PON

; One punch is initiated at the end of the path

N30 X90 SPN=4

; 4 punches initiated

N40 SPOF

N50 M2

[

Figure 12-7

Examples 3 and 4 for defined start of nibbling

Technologies

Function Manual, 10/2020, 6FC5397-8GP40-0BA1

275

Punching and nibbling

12.8 Examples

Examples 5 and 6 without defined start of nibbling

Example 5 Programming of SPP

Program code

Comment

N5 G0 X10 Y30

; Positioning

N10 X90 SPP=20 PON

; No defined start of nibbling,

; 4 punches initiated

N15 Y10

; One punch is initiated at the end of the path

N20 X10 SPP=20

; 4 punches initiated at intervals of 20 mm

N25 SPOF

N30 M2

Example 6 Programming of SPN

Program code

Comment

N5 G0 X10 Y30

; Positioning

N10 X90 SPN=4 PON

; No defined start of nibbling,

; 4 punches initiated

N15 Y10

; One punch is initiated at the end of the path

N20 X10 SPN=4

; 4 punches initiated

N25 SPOF

N30 M2

Technologies

276

Function Manual, 10/2020, 6FC5397-8GP40-0BA1

Punching and nibbling

12.8 Examples

Example 7 Application example of SPP programming

;

Figure 12-8

Workpiece

Extract from program:

Program code

Comment

N100 G90 X75 Y75 F60 PON

; Positioning to starting point (1) of the

; vertical line of holes, punch single hole

N110 G91 Y125 SPP=25 PON

; End point coordinates (incremental),

; path segment: 25 mm, activate punching

N120 G90 X150 SPOF

; Absolute dimensioning, position at

; the start point (2) of the horizontal line of

holes

N130 X375 SPP=45 PON

; End point coordinates, path segment: 45 mm

N140 X275 Y160 SPOF

; Positioning to starting point (3) of the

; oblique line of holes

N150 X150 Y75 SPP=40 PON

; End point coordinates, programmed

; path segment: 40 mm, calculated

; path segment: 37.39 mm

N160 G00 Y300 SPOF

; Positioning

Technologies

Function Manual, 10/2020, 6FC5397-8GP40-0BA1

277

Punching and nibbling

12.9 Data lists

12.9

Data lists

12.9.1

Machine data

12.9.1.1

General machine data

Number

Identifier: $MN_

Description

11450

SEARCH_RUN_MODE

Block search parameter settings

12.9.1.2

Channelspecific machine data

Number

Identifier: $MC_

Description

20150

GCODE_RESET_VALUES[n]

Reset G groups

26000

PUNCHNIB_ASSIGN_FASTIN

Hardware assignment for input-byte with stroke control

26002

PUNCHNIB_ASSIGN_FASTOUT

Hardware assignment for output-byte with stroke con-

trol

26004

NIBBLE_PUNCH_OUTMASK[n])

Mask for quick output bits

26006

NIBBLE_PUNCH_INMASK[n]

Mask for quick input bits

26008

NIBBLE_PUNCH_CODE[n]

Determination of the M functions

26010

PUNCHNIB_AXIS_MASK

Definition of punching and nibbling axes

26012

PUNCHNIB_ACTIVATION

Activation of punching and nibbling functions

26014

PUNCH_PATH_SPLITTING

Activation of automatic path segmentation

26016

PUNCH_PARTITION_TYPE

Behavior of single axes with active automatic path seg-

mentation

26018

NIBBLE_PRE_START_TIME

Automatically activated pre-initiation time

26020

NIBBLE_SIGNAL_CHECK

Monitoring of the input signal

12.9.2

Setting data

12.9.2.1

Channelspecific setting data

Number

Identifier: $SC_

Description

42400

PUNCH_DWELL_TIME

Dwell time

42402

NIBPUNCH_PRE_START_TIME

Pre-start time

42404

MINTIME_BETWEEN_STROKES

Minimum time interval between two consecutive

strokes

Technologies

278

Function Manual, 10/2020, 6FC5397-8GP40-0BA1

Punching and nibbling

12.9 Data lists

12.9.3

Language commands

G group

Language com-

Meaning

mand

SPOF

Stroke / Punch OFF

Punching and nibbling OFF

SON

Stroke ON

Nibbling ON

SONS

Stroke ON

Nibbling ON (position controller)

PON

Punch ON

Punching ON

PONS

Punch ON

Punching ON (position controller)

PDELAYON

Punch with Delay ON

Punching with delay ON

PDELAYOF

Punch with Delay OFF

Punching with delay OFF

Path segmentation

SPP

Path per stroke, modal action

SPN

Number of strokes per block, non-modal action

Technologies

Function Manual, 10/2020, 6FC5397-8GP40-0BA1

279

Table of contents

Preface

Introduction

1.1

About this documentation

Fundamental safety instructions

2.1

General safety instructions

2.2

Warranty and liability for application examples

2.3

Security information

Functional scope

3.1

Introduction

3.2

System overview

3.3

Function structure of tool management

3.4

Magazine management

3.5

Data structure HMI/PLC - NC (OPI)

3.6

PLC - NC interfaces

3.7

Access protection, protection levels

Basic commissioning and configuration

4.1

Input of the machine data

4.1.1

Settings with/without magazine management

4.1.2

Configuration via machine data

4.1.3

Additional settings

4.2

Configuration in SINUMERIK Operate

4.2.1

Function overview of the tool management editor

4.2.2

Editing the tool management

4.2.3

Parameterizing the tool management

4.2.3.1

Create tool unit

4.2.3.2

Define buffer locations

4.2.3.3

Define loading location

4.2.3.4

Create magazine configuration

4.2.3.5

Link assignments

Machine data

5.1

NC-specific machine data

5.2

Channel-specific machine data

5.3

Machine data for function replacement

100

5.4

Machine data for the Siemens user data

105

Tool management

Function Manual, 10/2020, 6FC5397-1HP40-0BA1

Table of contents

PLC programming

107

6.1

Overview

107

6.2

PLC description

108

6.2.1

Interfaces

108

6.2.2

Jobs from the NC tool management

111

6.2.3

Asynchronous transfer

113

6.2.4

Definitions of the acknowledgement status

113

6.2.5

Simplified acknowledgement of tool management commands

117

6.2.6

Diagnostics for communication between NC and PLC

118

6.2.7

Function blocks

121

6.2.8

Sample programs

122

6.3

Signal description of the PLC interface and transfer blocks

124

6.3.1

Overview of the blocks

124

6.3.2

Interface for loading/unloading magazine

125

6.3.3

Interface for spindle as change position

130

6.3.4

Interface for turrets as change position

136

6.3.5

Interface for loading/unloading magazine (multitool) (DB1071)

141

6.3.6

Interface for spindle (multitool) (DB1072)

142

6.3.7

Interface for turret (multitool) (DB1073)

146

6.3.8

Interface NC channels

150

6.3.9

Interface magazine configuration

151

6.3.10

Delete pending tasks

152

6.3.11

FC6: TM_TRANS2 - transfer block for tool management and multitool

153

6.3.12

FC7: TM_REV - transfer block for tool change with revolver

154

6.3.13

FC8: TM_TRANS - transfer block for tool management

157

NC programming

165

7.1

Overview of OPI and system variables

165

7.2

Use of the magazine data

168

7.3

Use of the tool and cutting edge data

170

7.4

Cutting edge data

172

7.4.1

Cutting edge data

172

7.4.2

Cutting edge parameter $TC_DP

172

7.4.3

User cutting edge data $TC_DPC

174

7.4.4

Cutting edge-related tool monitoring $TC_MOP

175

7.4.5

User cutting edge monitoring $TC_MOPC

176

7.4.6

Location of use-dependent offsets fine (additive offsets) $TC_SCP

176

7.4.7

Location-dependent offsets coarse (setting-up offsets) $TC_ECP

177

7.5

Tool data

179

7.5.1

Overview

179

7.5.2

Tool-related data $TC_TP

179

7.5.3

Tool-related grinding data $TC_TPG

185

7.5.4

Tool-related user data $TC_TPC

185

7.6

Magazine data

187

7.6.1

Overview of magazine data

187

7.6.2

Magazine description data $TC_MAP

187

7.6.3

Magazine user data $TC_MAPC

190

7.6.4

Magazine location data $TC_MPP

190

Tool management

Function Manual, 10/2020, 6FC5397-1HP40-0BA1

Table of contents

7.6.5

Magazine location user data $TC_MPPC

194

7.6.6

Magazine location type hierarchy $TC_MPTH

195

7.6.7

Distance to change position $TC_MDP

196

7.6.8

Magazine blocks $TC_MAMP

199

7.6.9

Assignment of buffers to spindles $TC_MLSR

206

7.7

Multitool data

209

7.7.1

$TC_MTP - multitool data

209

7.7.2

$TC_MTPP - Multitool location data

217

7.7.3

Multitool-related user data

222

7.7.4

Multitool-location-related user data

223

7.8

User-definable variables

224

7.9

NC language commands

226

7.9.1

CHKDNO - Uniqueness check for D number

226

7.9.2

CHKDM - Uniqueness check within a magazine

227

7.9.3

GETACTTD - Determining the tool number of a unique D No

228

7.9.4

GETDNO - Read out D numbers

229

7.9.5

SETDNO - Set or change D number

230

7.9.6

DZERO - Invalidate D numbers

230

7.9.7

DELDL - Delete additive offsets

231

7.9.8

NEWT - Create new tool

231

7.9.9

NEWMT Create new multitool

232

7.9.10

DELT Delete tool

234

7.9.11

DELMT - Delete multitool

234

7.9.12

$TC_MTPN - Delete one or all multitools

235

7.9.13

Reading the GETT - T no

236

7.9.14

SETPIECE - decrementing the workpiece counter

237

7.9.15

GETSELT - Read the selected T number

239

7.9.16

GETEXET - Reading of the loaded T number

242

7.9.17

$P_MTHSDC - master tool holder with regard to the D offset selection

245

7.9.18

$P_TH_OF_D - master tool holder to which the current D offset refers

247

7.9.19

GETACTT - Read the active internal T number

248

7.9.20

SETMS - Set master spindle

250

7.9.21

SETMTH - Set master toolholder number

250

7.9.22

POSM - Positioning the magazine

253

7.9.23

POSMT - position multitool on toolholder to location number

255

7.9.24

MVTOOL - NC command to move tool

258

7.9.25

SETTA - Activate tool from wear group

261

7.9.26

SETTIA - Deactivate tool from wear group

263

7.9.27

RESETMON - NC command for setpoint activation

265

7.9.28

DELTC - Delete toolholder data record

269

7.9.29

TCA - tool selection/tool change irrespective of tool status

270

7.9.30

TCI - Load tool from buffer into magazine

273

7.9.31

GETFREELOC - Search for empty location

275

7.9.32

DELMLRES - Delete location status "reserved for tool in the buffer"

281

7.9.33

DELMLOWNER - Delete owner magazine location of the tool

282

7.9.34

$P_USEKT - Tool change only with tools of subgroup

284

7.9.35

TOOLGNT/TOOLGT - Tool groups

287

7.9.36

$P_TMNOIS - is number, T number, magazine number, or MT number

288

7.9.37

$P_TOOLEXIST - Determine existence of a tool

289

7.9.38

$A_TOOLMN - read magazine no. from tool

290

7.9.39

$P_MTOOLN / $P_MTOOLMT- determine number of multitools / MT number

291

Tool management

Function Manual, 10/2020, 6FC5397-1HP40-0BA1

Table of contents

7.9.40

$P_MTOOLNT / $P_MTOOLT - Number of tools in the multitool

292

7.9.41

$A_TOOLMLN - Read magazine location No. of tool

293

7.9.42

$P_TOOLND - Read number of cutting edges for tool

294

7.9.43

$A_MONIFACT - factor for tool life monitoring

294

7.9.44

$AC_MONMIN - Factor for tool search

296

7.9.45

$P_TOOLNG - Number of tool groups

299

7.9.46

$A_MYMN / $A_MYMLN - Owner magazine/location of the tool

299

7.9.47

$A_MYMTN / $A_MYMTLN - $A_TOOLMTN / $A_TOOLMTLN - tools in multitool

300

7.9.48

$P_TOOLNT / $P_TOOLT - T numbers

302

7.9.49

$P_TOOLD - D numbers

302

7.9.50

$P_TOOLNDL - Number of defined DL offsets

303

7.9.51

$A_USEDND - Workpiece counting

304

7.9.52

$A_USEDT - Workpiece counting

305

7.9.53

$A_USEDD - Workpiece count

306

7.9.54

$A_TOOLADAPT - Assignment of tool to adapter

307

7.9.55

$TC_ADPTx - adapter description

308

7.9.56

$P_MAGNA / $P_MAGA - Tool adapter

310

7.9.57

$P_MAGN / $P_MAG - Magazine

311

7.9.58

$P_MAGNDIS / $P_MAGDISS / $P_MAGDISL - magazine distance tables

312

7.9.59

$P_MAGNS / $P_MAGS - Toolholder

313

7.9.60

$P_MAGNREL / $P_MAGREL - Assigned buffer

314

7.9.61

Example of magazine configuration system variables

315

7.9.62

$P_MAGNH / $P_MAGNHLT / $P_MAGHLT - Location type hierarchies

317

7.9.63

Additional language commands

320

7.9.64

Variables for subroutine replacement technique

327

7.9.65

Variables for tool change in synchronized action

328

7.10

Definitions when programming data

330

7.10.1

Tool change

330

7.10.2

Cutting edge selection

331

7.10.3

Tool transfer from program test

332

7.11

Programming T=location number

333

7.12

Call multiple turrets with "T=location number"

335

7.13

Programming examples

336

7.14

Overview of the remaining OPI blocks of tool management

337

7.14.1

Magazine data, directory

337

7.14.2

Tool data, directory

337

7.14.3

Parameterization, return parameters _N_TMGETT, _N_TSEARC

338

7.14.4

Working offsets

339

7.14.5

PI services and language commands for tool management

339

Description of functions

345

8.1

Magazines

345

8.1.1

Magazine configuration

345

8.1.2

Magazine types

346

8.1.3

Loading magazine

347

8.1.4

Buffer

348

8.1.5

Box-type and chain magazines

349

8.1.6

Circular magazine

352

8.1.7

Other magazine types

353

8.1.8

Wear group

354

Tool management

Function Manual, 10/2020, 6FC5397-1HP40-0BA1

Table of contents

8.1.9

Background magazine

355

8.1.10

Consider adjacent location

356

8.2

359

8.2.1

Loading sequence

359

8.2.2

Function of the PLC when loading?

361

8.2.3

Loading by directly assigning the T number

364

8.2.4

Load tools via a part program

364

8.2.5

Retroload tool data

365

8.3

Unloading

368

8.3.1

Unloading sequence

368

8.3.2

PLC function when unloading

369

8.3.3

Unloading by deleting the T number from the magazine location

372

8.4

Tool change box-type, chain, circular magazines

373

8.4.1

Overview

373

8.4.2

General tool change sequence

374

8.4.3

Preparing a tool change via T command

378

8.4.4

Execution of the tool change

379

8.4.5

Tool change for chain and box-type magazines

380

8.4.5.1

PLC function during preparation (chain, box type)

380

8.4.5.2

PLC function during tool change (chain, box type)

383

8.4.5.3

PLC sample programs tool change

386

8.4.5.4

Example structure of the PLC program for a tool change

388

8.4.6

Tool change with turret

390

8.4.7

Selecting a tool and a cutting edge

391

8.4.8

Predecoding (preprocessing) and block execution (main run)

393

8.4.9

Traverse axes while tool is being changed

395

8.4.10

Special cases "T0", empty spindle, multiple T selection

395

8.4.11

Number of replacement tools

396

8.4.12

Tool changing errors

397

8.4.13

Monitoring the maximum speed of a tool

398

8.4.14

Tool changes in the NC using synchronized actions

404

8.4.15

Replacing functions with subprograms

407

8.4.15.1

Function replacement

407

8.4.15.2

Replacement of the TCA command

411

8.4.16

Block search

413

8.4.17

Block search (SSL) in conjunction with active tool management

415

8.4.18

System variables for state before block search

418

8.4.18.1

Description of the variables

418

8.4.18.2

Example

419

8.4.19

Program test

422

8.4.20

Several spindles in one channel or TO unit

424

8.4.21

Decoupling the tool management from the spindle number

425

8.4.22

Several spindles/toolholders

430

8.4.23

Several magazines in one channel or one TO unit

431

8.4.24

Reset and start mode

431

8.4.25

Repeating a tool change with the same tool identifier

438

8.5

Relocating tools and positioning the magazine

442

8.5.1

Relocating sequence

442

8.5.2

Relocation by the PLC

444

8.5.3

Positioning the magazine

447

Tool management

Function Manual, 10/2020, 6FC5397-1HP40-0BA1

Table of contents

8.6

Several tools at a magazine location (multitool)

450

8.6.1

Brief description

450

8.6.2

Programming

453

8.6.3

Tool change with a tool from a multitool

454

8.6.4

Tool change and tool number for multitools

460

8.7

Using manual tools

470

8.7.1

Manual tools (adding tools during machining)

470

8.7.2

Tool change with manual tools

474

8.7.3

Role of the PLC for manual tools

476

8.8

Search for tool

480

8.8.1

Strategies for tool searches

480

8.9

Empty location search

483

8.9.1

Empty location search for a tool - from spindle to magazine

483

8.9.2

Search strategy for empty locations

484

8.9.3

Search procedure for empty locations

485

8.9.4

Search strategy, 1:1 exchange (old for new)

485

8.9.5

Tool search in wear group

487

8.10

Location type hierarchies

491

8.10.1

Hierarchies of location types in magazines

491

8.10.2

Conventional location type hierarchy $TC_MAMP2, Bit15=0

493

8.10.3

Alternative location type hierarchy $TC_MAMP2, Bit15=1

494

8.10.4

Search strategy across magazines

496

8.10.5

Mini hierarchies

497

8.11

Tool monitoring (workpiece count, tool life, wear)

499

8.11.1

Monitoring types

499

8.11.2

Tool life monitoring

502

8.11.3

Workpiece count monitoring

503

8.11.4

Wear monitoring

504

8.11.5

Signals to and from the PLC

506

8.12

Tool monitoring without active tool management

510

8.12.1

Tool monitoring overview

510

8.12.2

Tool life monitoring

511

8.12.3

Workpiece count monitoring

512

8.12.4

Wear monitoring

513

8.12.5

Monitoring the additive offset

513

8.12.6

Working with replacement tools

513

8.12.7

Examples

513

8.12.8

NC language commands

514

8.13

Variants of D-number assignments

515

8.13.1

Free selection of D numbers for every T

515

8.13.2

Location-dependent offsets (additive offsets)

517

8.14

Tool adapter

520

8.14.1

Machine data for setting adapters of type 1 and type 2

520

8.14.2

Creating/deleting adapters

520

8.14.3

Constraints for adapters

521

8.14.4

Managing adapter data

522

8.14.4.1

Managing adapter data for type 1 and type 2

522

8.14.5

Adapter type 1

522

Tool management

Function Manual, 10/2020, 6FC5397-1HP40-0BA1

Table of contents

8.14.5.1

Overview

522

8.14.5.2

Description of function

523

8.14.5.3

Activation

524

8.14.5.4

Adapter data $TC_ADPT

533

8.14.5.5

Transformed data of the active tool $P_ADT[n]

534

8.14.6

Adapter type 2 (angle head adapter) (option)

534

8.14.6.1

Assigning an angle head adapter

534

8.14.6.2

Angle head adapter - tool and adapter separate (type 2)

535

8.14.7

Offset values

541

8.14.7.1

Base length for the adapter

541

8.14.7.2

Cutter radius compensations and setup offsets for adapters

542

8.14.7.3

Cutting edge data for the orientation type 2 adapter

542

8.14.8

OPI block ADN

543

8.15

Power failure while tool command is in progress

545

SINUMERIK Operate user interface

547

9.1

Configuring the user interface

547

9.1.1

General settings

550

9.1.2

Configuring tool lists

555

9.1.2.1

Tool parameter identifiers

559

9.1.2.2

Cutting edge parameter identifiers

561

9.1.2.3

Monitoring parameter identifiers

564

9.1.2.4

Grinding parameter identifiers

565

9.1.2.5

Magazine location parameter identifiers

566

9.1.2.6

Magazine location adapter parameter identifiers

567

9.1.2.7

Multitool parameter identifiers

567

9.1.2.8

Multitool location parameter identifiers

568

9.1.3

Configuring list parameters

569

9.1.4

List of tool types

573

9.1.5

Configure tool types

575

9.1.6

Configuring the "Additional Data" window

577

9.1.7

Configure the "New tool - favorites" window

579

9.1.8

Configuring the "New Tool" window

579

9.1.9

Configuring the "New Multitool" window

580

9.1.10

Configuring the "New Tool from Code Carrier" window

580

9.1.11

Configuring the "New Tool from File" window

581

9.1.12

Configuring default values for new tools

581

9.1.13

Configuring the "Details" window

586

9.1.14

Assigning a name for magazines and magazine locations

587

9.1.15

Configuring the "Assign Tooltips for Multitool Locations" window

589

9.1.16

Assigning a name for magazine location types

590

9.1.17

Assignment of magazines and magazine locations to channels

591

9.1.18

Assignment between magazines and magazine locations and coordinate systems

593

9.1.19

Disabling the softkey depending on filters

594

9.1.20

Configuring the "Load Station Selection" window

595

9.1.21

Coolant and tool-specific functions

596

9.1.22

Reason for the tool change when reactivating

599

9.1.23

Configure the code carrier connection

603

9.1.24

Configuring Save to file

606

9.2

Creating OEM texts

608

9.2.1

Identifiers of the standard texts

609

Tool management

Function Manual, 10/2020, 6FC5397-1HP40-0BA1

Table of contents

9.2.2

Examples of OEM texts

611

9.3

Examples

614

9.3.1

Example: Configuring an OEM tool list

614

9.3.1.1

Adapting the configuration file

614

9.3.1.2

Adaptation of the customer text file

616

9.3.2

Example: Configuring magazine location types with names

618

9.3.2.1

Adapting the configuration file

618

9.3.2.2

Adaptation of the customer text file

619

9.4

Working with two tool holders

622

Code carrier connection - Tool Ident Connection (option)

625

10.1

Installation

625

10.1.1

System requirements

625

10.1.2

Installation of Tool Ident Connection

626

10.1.2.1

Activation of Tool Ident Connection

626

10.1.2.2

Installation of Wkonvert wizard

627

10.2

Configuration

633

10.2.1

Configuration schematic

633

10.2.2

Configuration of the tool lists

633

10.2.3

TDIIdentCfg.xml

633

10.2.4

Read/write device at the PLC

636

10.2.5

Data conversion

637

10.2.5.1

Using the Wkonvert wizard

639

10.2.5.2

Messages of the Wkonvert wizard

640

10.2.6

Conversion files wkonvert.txt and DefToolDat.txt

641

10.2.6.1

Structure of the description file wkonvert.txt

641

10.2.6.2

Examples for the description files wkonvert.txt

646

10.2.6.3

Tool data initialization file DefToolDat.txt

649

10.2.7

Conversion rule based on the MCIS-C script language

651

10.2.7.1

Structure of the conversion rule

651

10.2.7.2

Access to tool data

653

10.2.7.3

Auxiliary functions for numerical coding

655

10.2.7.4

Configuration of ToolSpec.xml

661

10.2.7.5

Error handling

662

10.2.7.6

Description of the MCIS-C script language

663

10.2.7.7

Help functions in conversion specifications

664

10.2.8

Examples

665

10.3

PLC interface in the DB19

670

10.3.1

Structure

670

10.3.2

Function call of the PLC interface

670

10.3.3

Assignment of the PLC for transfer parameters

671

10.3.4

Assignment of the PLC for return values

672

10.3.5

Executing functions

672

10.3.5.1

General sequence when executing functions

672

10.3.5.2

Pulse diagram for positive execution of a function

673

10.3.5.3

Pulse diagram when negative execution of a function

674

10.3.5.4

Pulse diagram "Ident_Ready" signal

674

10.3.6

PLC interface for the Parameter operating area

675

10.3.6.1

Assignment of the PLC interface for the Parameter area

675

10.3.6.2

Load the tool

676

Tool management

Function Manual, 10/2020, 6FC5397-1HP40-0BA1

Table of contents

10.3.6.3

Sequence

677

10.3.6.4

Sequence when canceled by the PLC

678

10.3.6.5

Unloading a tool

679

10.3.6.6

Diagnostics

679

10.3.6.7

Restrictions

681

10.3.6.8

Error messages

681

10.3.7

PLC data types

681

10.4

Command codes

683

10.4.1

Functional scope of the PLC interface (K codes)

683

10.4.2

Parameter description

683

10.4.3

Loading from the code carrier (K code = 0)

684

10.4.4

Unload to code carrier (K code = 1)

685

10.4.5

Loading of production host computer (K code = 4)

686

10.4.6

Unload to the production host computer (K code = 5)

687

10.4.7

Loading a tool from the tool list (K code = 7)

688

10.4.8

Unloading a tool in the tool list (K code = 8)

689

10.4.9

Empty location search (K code = 9)

690

10.4.10

Delete tool in NC (K code = 10)

691

10.4.11

Updating the code carrier (K code = 14)

692

10.4.12

Reading data from the code carrier (K code = 15)

693

10.4.13

Error codes

694

10.5

Examples

700

10.5.1

Loading the code carrier via PLC interface

700

10.5.2

Unloading to the code carrier via PLC interface

703

Alarms

705

11.1

Overview

705

11.2

Alarm description

708

Appendix

741

A.1

List of abbreviations

741

A.2

Documentation overview

743

A.3

Available IPCs

744

Index

745

Tool management

Function Manual, 10/2020, 6FC5397-1HP40-0BA1

Introduction

1.1

About this documentation

This documentation is part of the documentation category of SINUMERIK Function Manuals.

SINUMERIK Function Manuals

The SINUMERIK Function Manuals describe the NC functions of a SINUMERIK control.

The target group are configuring engineers, technologists, commissioning engineers and

programmers.

Each Function Manual covers a specific topic and contains all the function descriptions for this

topic.

The following table shows which Function Manuals are available for your SINUMERIK control and

which topics a Function Manual covers:

Function Manual

Topic

Basic functions

Basic functions of a CNC control

Axes and spindles

Axis and spindle functions, axis couplings

Transformations

Transformation functions

Monitoring and compensating

Axis monitoring and compensation functions, collision avoid-

ance

Tools

Functions for selection, correction and monitoring of tools

Synchronized actions

Functionality of synchronized actions

PLC

Structure and functions of the PLC

Tool management

Function, commissioning and programming of tool manage-

ment

Technologies (for SINUMERIK ONE

Extended technological functionalities

and SINUMERIK 840D sl only)

Overview of contents

You will find an overview of the main chapters of the descriptions of functions that are contained

in a Function Manual on the title page.

Validity

The title page also contains all data about the validity of a document, i.e. for which SINUMERIK

control and for which software version this edition of the Function Manual is valid.

Tool management

Function Manual, 10/2020, 6FC5397-1HP40-0BA1

Introduction

1.1 About this documentation

System data

In the descriptions of functions, the system data relevant for a function (machine data, setting

data, system variables, interface signals and alarms) are only described with the level of detail

that is strictly necessary to understand the function. You will find detailed information on this

data in the relevant List Manuals and for alarms in the Diagnostics Manual.

PLC blocks

The descriptions of functions often refer to the PLC function blocks (FB) and functions (FC). The

descriptions of these blocks apply to the SINUMERIK 840D sl and can only be applied in part to

other SINUMERIK controls.

Interface signals

In this document, only the absolute address valid for the SINUMERIK 840D sl is used to address

interface signals.

General graphical conventions

Examples

<signal address> (<signal name>)

DB31, ... DBX16.0-2 (actual gear stage A to C)

DB31, ... DBX16.3 (gear is changed)

Note

Quantity structure

Explanations concerning the NC/PLC interface are based on the absolute maximum number of

the following components:

• Mode groups (DB11)

• Channels (DB21, etc.)

• Axes/spindles (DB31, etc.)

Tool management

Function Manual, 10/2020, 6FC5397-1HP40-0BA1

Fundamental safety instructions

2.1

General safety instructions

WARNING

Danger to life if the safety instructions and residual risks are not observed

If the safety instructions and residual risks in the associated hardware documentation are not

observed, accidents involving severe injuries or death can occur.

• Observe the safety instructions given in the hardware documentation.

• Consider the residual risks for the risk evaluation.

WARNING

Malfunctions of the machine as a result of incorrect or changed parameter settings

As a result of incorrect or changed parameterization, machines can malfunction, which in turn

can lead to injuries or death.

• Protect the parameterization against unauthorized access.

• Handle possible malfunctions by taking suitable measures, e.g. emergency stop or

emergency off.

Tool management

Function Manual, 10/2020, 6FC5397-1HP40-0BA1

Fundamental safety instructions

2.2 Warranty and liability for application examples

2.2

Warranty and liability for application examples

Application examples are not binding and do not claim to be complete regarding configuration,

equipment or any eventuality which may arise. Application examples do not represent specific

customer solutions, but are only intended to provide support for typical tasks.

As the user you yourself are responsible for ensuring that the products described are operated

correctly. Application examples do not relieve you of your responsibility for safe handling when

using, installing, operating and maintaining the equipment.

Tool management

Function Manual, 10/2020, 6FC5397-1HP40-0BA1

Fundamental safety instructions

2.3 Security information

2.3

Security information

Siemens provides products and solutions with industrial security functions that support the

secure operation of plants, systems, machines and networks.

In order to protect plants, systems, machines and networks against cyber threats, it is necessary

to implement - and continuously maintain - a holistic, state-of-the-art industrial security

concept. Siemens’ products and solutions constitute one element of such a concept.

Customers are responsible for preventing unauthorized access to their plants, systems,

machines and networks. Such systems, machines and components should only be connected to

an enterprise network or the internet if and to the extent such a connection is necessary and only

when appropriate security measures (e.g. firewalls and/or network segmentation) are in place.

For additional information on industrial security measures that may be implemented, please

visit

https://www.siemens.com/industrialsecurity https://www.siemens.com/industrialsecurity ).

Siemens’ products and solutions undergo continuous development to make them more secure.

Siemens strongly recommends that product updates are applied as soon as they are available

and that the latest product versions are used. Use of product versions that are no longer

supported, and failure to apply the latest updates may increase customer’s exposure to cyber

threats.

To stay informed about product updates, subscribe to the Siemens Industrial Security RSS Feed

under

https://www.siemens.com/industrialsecurity https://new.siemens.com/global/en/products/

services/cert.html#Subscriptions).

Further information is provided on the Internet:

Industrial Security Configuration Manual (https://support.industry.siemens.com/cs/ww/en/

view/108862708)

WARNING

Unsafe operating states resulting from software manipulation

Software manipulations, e.g. viruses, Trojans, or worms, can cause unsafe operating states in

your system that may lead to death, serious injury, and property damage.

• Keep the software up to date.

• Incorporate the automation and drive components into a holistic, state-of-the-art industrial

security concept for the installation or machine.

• Make sure that you include all installed products into the holistic industrial security concept.

• Protect files stored on exchangeable storage media from malicious software by with suitable

protection measures, e.g. virus scanners.

• On completion of commissioning, check all security-related settings.

Tool management

Function Manual, 10/2020, 6FC5397-1HP40-0BA1

Functional scope

3.1

Introduction

Overview

The "Tool management" (TOOLMAN) function ensures that at any given time the correct tool is

selected and that the data assigned to the tool is up to date. The function is used on machine

tools with circular magazines, chain magazines or box magazines. Tool management also

enables the following functions:

• Optimum tool staging for tool change.

• Avoidance of waste by monitoring tool operation (function "Tool monitoring function").

• Avoidance of machine downtimes by using replacement tools.

• Search for a suitable magazine location for the tool being replaced (with function Magazine

management).

Note

If only "TMMO" is active, magazine management must be implemented by the machine

manufacturer in the PLC user program.

Function versions of tool management

There are 3 different function versions when handling tools:

• TMMO: ToolManagement Tool (Monitoring)

(English: TMMO = Tool Management Tool Monitoring)

• TMMG: ToolManagementMagazines (only available with active tool management)

(English: TMMG = Tool Management Magazines)

• TMMO and TMMG

Combination of the two function types

Quantity structure

NCU 730

NCU 720

NCU 710

Number of magazines

Number of cutting edges

3000

1500

Number of tools per multitool

Tool management

Function Manual, 10/2020, 6FC5397-1HP40-0BA1

Functional scope

3.2 System overview

3.2

System overview

The following diagram shows an overview of tool management.

6\VWHP VWUXFWXUH

+0,

7',

70 6HUYLFH

&RGH FDUULHU

23, LQWHUIDFH

,QWHUIDFH

3/&

/DQJXDJH

%DVLF SURJUDP

8VHU SURJUDP

GDWD PDQDJH

3/&

PHQW

8VHU LQWHUIDFH

VHTXHQWLDO

FRQWURO V\VWHP

ORJLF

Figure 3-1

System overview diagram Tool management

Magazine management

Special functions of the tool management include magazine management, tool and empty

location search. These additional functions are only available when tool management is active.

Without active tool management, the magazine management must be implemented by the

machine manufacturer in the PLC user program.

Tool monitoring

The tool monitoring function is used to monitor tool lifetime, unit quantity or wear values.

Tool management

Function Manual, 10/2020, 6FC5397-1HP40-0BA1

Functional scope

3.2 System overview

OPI variables

Additional functions are available using OPI variables on the PLC or HMI side. You can use OPI

variables (NC variables) by choosing them with the NC-VAR selector.

Further information

• SINUMERIK 840D sl: Function Manual PLC

System variables

NC programs (e.g. cycle, ASUB) provide corresponding NC commands to achieve optimum

adaptation of the tool management to the machine environment. You can obtain a clear

overview about the data structures that form the basis of the tool management. They are

represented in the form of NC data blocks.

Operator panels

The following operator panels can be used for tool management:

• OP177, e.g. for loading magazines

• OP8T, e.g. for box-type magazines

Data

Data storage and management is carried out in the NC and SINUMERIK Operate. All data can be

read and written manually via the NC program or by data transfer.

Operation via system screens

Operation is mainly performed via system screens. There are system screens for commissioning

and for tool management operation (magazine lists, tool lists, loading/unloading).

Configuration of user-specific screens

Tool-specific data that is not displayed via SINUMERIK Operate system screens can be displayed

and changed in configurable user-specific screens.

The configuration of user-specific screens is described in:

Further information

• SINUMERIK 840D sl: Commissioning Manual, Base Software and Operating Software;

SINUMERIK Integrate Run MyScreens (BE2)

Programming in the NC part program

The tool management function makes it possible to call a tool in the part program using a name

(identifier), e.g. T = "end mill 120 mm".

Tool call is still possible via the T no. (tool number). The T no. is then the name of the tool

(e.g. T=T12345678).

Tool management

Function Manual, 10/2020, 6FC5397-1HP40-0BA1

Functional scope

3.2 System overview

A tool is uniquely defined by its internal T number or identifier and its duplo number.

Furthermore, each tool can be uniquely identified by its name. The internal T number

is generally assigned by the NC, and is not used for programming a tool change in the part

program.

Using a machine data, it can be set as to whether the change is realized using the T command

(typical for lathes) or whether the tool is prepared using T programming and only changed with

M06. This machine data setting is independent of the magazine type.

The following characters are permitted for the identifier:

[ _ ] [ a...z ] [ A...Z ] [ 0...9 ] ; [ + - . , ]

Identifiers are case-sensitive, i.e. differentiate between upper-case and lower-case characters.

PLC

There are data blocks (DB71-73) as well as DB1071-1073 for receiving tool management

commands and function blocks (FC6, FC7, FC8) for acknowledging the tool management

commands. A "fast acknowledgement" is implemented for simple applications in data blocks

DB71...73.

Another block, FC22, is used as a direction selection for magazines.

Tool management data can also be read and written via FB2 and FB3. Complex tool management

services can be initiated via FB4.

Location coding

Fixed location coding as well as variable location coding are supported for the tools.

Location type

The location type defines the type and shape of the location. By assigning location types to

magazine locations it is possible to subdivide a magazine into areas. This means that different

types of special tools, e.g. "especially_large", "especially_heavy" can be assigned to specific

locations.

The location types can be placed in ascending order - a so called hierarchy. This order determines

that a tool that is supposed to be inserted in a "small" location type can also be placed in a "larger"

location type if no "smaller" location type is vacant.

Monitoring functions

In tool management, it is possible to select either workpiece counts or tool life monitoring (with

reference to the cutting edges). Further, a wear monitoring function is available. Replacement

tools (duplo tools) are differentiated by means of a duplo number.

Search strategy

Various strategies are possible for tool search and to search for the empty location of the "old

tool". The "old tool" is the tool to be replaced.

The empty location search strategy is used for loading tools.

Tool management

Function Manual, 10/2020, 6FC5397-1HP40-0BA1

Functional scope

3.2 System overview

Tool groups

Tools with the same identifier are combined in tool groups. Using duplo numbers, a distinction

can be made between tools - and used as replacement tools ("sister tool") within the framework

of the tool management.

Excerpt from TOOLMAN basic data

Term

Data/Range

Magazine configuration per channel

Total number of magazines

Max. 64

Total number of magazine locations

Max. 1500

Total number of tools

Across all TO units max. 1500

Programming tools (names) in the NC program us-

e.g. T="angled mill_32"

ing 32 alphanumeric characters

Duplo number¹⁾

1 - 32000

Total number of cutting edges

Max. 3000

Location type definition

Assigning location types to magazine locations

Viewing adjacent locations in half locations

2dimensional

Location coding

Fixed or variable

Strategy for tool search

can be set (programmable) via system variables

Strategy for empty location search

can be set (programmable) via system variables

M06 command for tool change

M code, settable via MD, channel-specific

Tool change with M06 or T command

settable via MD, channel-specific

Wear monitoring

For every cutting edge

Wear monitoring according to tool life

Resolution in ms

Wear monitoring according to number of workpie-

Counter

ces

Access to tool management data via NC program

System variables

Automatic decoding stop until tool is selected

Yes

T=Location No.

settable via MD

1) The duplo number or the duplo tool is called "sistertool" in SINUMERIK Operate.

Tool management

Function Manual, 10/2020, 6FC5397-1HP40-0BA1

Functional scope

3.3 Function structure of tool management

3.3

Function structure of tool management

HMI

• Tool list

• Tool wear list

• OEM tool list

• Magazine list

• Tool data management

- State

- Monitoring

- Corrections

• Magazine data management

- Magazines

- Magazine locations

• Tool management

- Search for tool

- Find empty location

- Change tool

- Load, unload

PLC

• Magazine control

• Gripper control

• Spindle control

• Safety interlocks

• Execute tool change

• Calculation of position, if necessary

• Own change strategy, if applicable

Tool management

Function Manual, 10/2020, 6FC5397-1HP40-0BA1

Functional scope

3.4 Magazine management

3.4

Magazine management

Tool magazine management - TMMG

Magazine management administers the magazine locations. The locations have the following

properties:

• The locations are free.

• The locations are occupied with tools.

• These locations are occupied by oversized tools in adjacent locations.

• The locations are reserved for a tool in a buffer or loading magazine.

The tool magazine management offers the following functions:

• Magazine management provides extended functions such as load, unload, position tools or

position magazines.

• It also includes search functions for tools, magazine locations, and search strategies for

replacement tools.

• For the tool monitoring functions, while the activated monitoring is running, tools are

disabled and no longer used.

• For further machining, if a similar tool (replacement tool) is present which is not disabled,

then this tool is used automatically.

• When tool management is active, you define the configuration of magazines, loading

magazines, spindles, grippers, etc. The NC defines the interfaces (DB 71 to DB 73) in the PLC

via the configuration data.

Task-related tool motions (e.g. position chain, swivel gripper) are derived from the interface

processing. After tool movements, the positions and task status should be acknowledged via

basic program blocks (FC6, FC7 and FC8). The acknowledgement procedure is described in

detail in Definitions of the acknowledgement status (Page 113) and Simplified

acknowledgement of tool management commands (Page 117).

If necessary, create another cycle (or ASUP) for the NC program where tool changing is

programmed with the required travel motions. An identifier is programmed for the tool change

or tool preselection when the TOOLMAN system is active. A duplo number is also available to

support unique identification of replacement tools. Tool identifier and duplo numbers are always

mapped on an internally assigned T number. This internally assigned T number is used for

addressing the variables described in the following.

Magazine types in the magazine management

Magazine management manages the following real magazines.

• Circular magazine (Page 352)

• Box-type and chain magazines (Page 349)

Other magazine types, e.g. pick-up magazines, are mapped onto these.

Real magazines can be defined as a circular, chain or box-type. Loading points or loading stations

shall be used as the magazine type for loading and unloading.

A magazine buffer combines all other locations in which tools can be placed (spindle, gripper, ...).

Tool management

Function Manual, 10/2020, 6FC5397-1HP40-0BA1

Functional scope

3.6 PLC - NC interfaces

3.6

PLC - NC interfaces

Overview

The core of the tool management is located on the NC. The PLC merely contains the interfaces

for the machine-specific part.

3/&

3DUDPH

WHUV

/RDGLQJ

DVVLJQPHQW

0DFKLQH

XQORDGLQJ VW

EXIIHU HWF

GDWD

/RDGLQJ XQO

RDGLQJ VW

72 GDWD

6SLQGOH

7RRO PDQDJH

%DVLF

PHQW

SURJUDP

6SLQGOH

0DJD]LQH

GDWD

7XUUHW

/RF WRRO ROG

70B75$16

/RF WRRO QHZ

70B',5

6HWSRLQW SRV

'LUHFWLRQ

6HOHFWLRQ RI

$FWXDO SRV

'LVWDQFH WR JR

GLUHFWLRQ

Figure 3-2

Data structure and PLC - NC interface

Tool management

Function Manual, 10/2020, 6FC5397-1HP40-0BA1

Functional scope

3.7 Access protection, protection levels

3.7

Access protection, protection levels

The access to programs, data and functions is protected via 8 hierarchical levels according to

customer requirements. These are subdivided into

• Four password levels for Siemens, machine manufacturers and end users

• Four keyswitch positions for end users

Protec-

Locked by:

User

tion level

Password

Siemens

Password

Machine manufacturer: Development

Password

Machine manufacturer: Commissioning engineer

Password

End user: Service

Keyswitch, position 3

End user: Programmer, machine setter

Keyswitch, position 2

End user: Qualified operator, who does not program

Keyswitch, position 1

End user: Selected operator, who does not program

Keyswitch, position 0

End user: Semi-skilled operator

Examples of functions that can be disabled with SINUMERIK Operate:

• Loading

• Unloading

• Magazine list, tool list display

• Tool cabinet, tool catalog

• Loading the magazine configuration

Tool management

Function Manual, 10/2020, 6FC5397-1HP40-0BA1

Basic commissioning and configuration

4.1

Input of the machine data

4.1.1

Settings with/without magazine management

Setting without magazine management

Make the following settings if you are commissioning the tool management without NC

magazine management:

MD18080 $MN_MM_TOOL_MANAGEMENT_MASK

Memory for the tool management is re-

(Page 63)

served step by step (SRAM).

= 02H

Bit 1

Provide monitoring data.

MD20310 $MC_TOOL_MANAGEMENT_MASK (Page 91)

Activating the tool management func-

tions.

= 02H

Bit 1

Monitoring functions of tool management active.

MD17530 $MN_TOOL_DATA_CHANGE_COUNTER

Marking the changed tool data for HMI.

(Page 58)

= 1FH

Bit 0

Tool status change.

Bit 1

Tool remaining unit quantity change.

Bit 2

Tool data change service.

Bit 3

Magazine data in the change service.

Bit 4

ISO data in the change service.

MD28450 $MC_MM_TOOL_DATA_CHG_BUFF_SIZE

Buffer for changing tool data (DRAM).

= 400

Number of entries in the buffer for the OPI change service for tool data. Dynamic memory is

used. This buffer is only created if either bit 2 or bit 3 is set in MD17530 $MN_TOOL_DA-

TA_CHANGE_COUNTER (default setting).

Tool management

Function Manual, 10/2020, 6FC5397-1HP40-0BA1

Basic commissioning and configuration

4.1 Input of the machine data

Setting with magazine management

Make the following settings if you are commissioning the tool management with NC magazine

management:

MD18080 $MN_MM_TOOL_MANAGEMENT_MASK

Memory for the tool management is re-

(Page 63)

served step by step (SRAM).

= 03H

Bit 0

Provide tool management data.

Bit 1

Provide monitoring data.

MD20310 $MC_MM_TOOL_MANAGEMENT_MASK

Activating the tool management func-

(Page 91)

tions.

= 03H

Bit 0

Magazine management active.

Bit 1

Monitoring functions of tool management active.

MD17530 $MN_TOOL_DATA_CHANGE_COUNTER

Marking the changed tool data for HMI.

(Page 58)

= 1FH

Bit 0

Tool status change.

Bit 1

Tool remaining unit quantity change.

Bit 2

Tool data change service.

Bit 3

Magazine data in the change service.

Bit 4

ISO data in the change service.

MD28450 $MC_MM_TOOL_DATA_CHG_BUFF_SIZE

Buffer for changing tool data (DRAM).

= 400

Number of entries in the buffer for the OPI change service for tool data. Dynamic memory is

used. This buffer is only created if either bit 2 or bit 3 is set in MD17530 $MN_TOOL_DA-

TA_CHANGE_COUNTER (default setting).

SINUMERIK 840D sl. Service - Functions. Manual (2018-2020) - page 81