Content      ..     5      6      7      8     ..

SINUMERIK 840D sl/828D. Job Planning. Programming Manual (2010-2018) - page 7

Tool offsets

11.5 3D tool radius compensation

The position of the machining point on the peripheral surface of the tool is set with the insertion

depth.

① Programmed path

② Milling tool machining point

③ Milling tool reference point

④ Milling tool tip

ISD

Insertion depth (InSertion Depth)

Figure 11-2

Insertion depth

Tool radius compensation referred to a differential tool

3D TRC for circumferential milling referred to a differential tool is activated via the CUT3DCD

command. It should be applied if the programmed contour refers to the center-point path of a

standard tool, and a tool other than a differential tool is used for machining. When calculating

the 3D tool radius compensation, only the wear value of the radius of the active tool

($TC_DP15) and any programmed tool offsets OFFN and TOFFR are taken into account. The

basic radius ($TC_DP6) of the active tool is not taken into account.

Pocket milling with inclined side walls for circumferential milling with CUT3DC

In this 3D tool radius compensation, a deviation of the mill radius is compensated by infeed

toward the surface normals to be machined. The plane, in which the milling tool face is located,

remains unchanged if the insertion depth ISD has remained the same. For example, a milling

tool with a smaller radius than a standard tool would not reach the pocket base, which is also

the limitation surface. For automatic tool infeed, this limitation surface must be known to the

control, see Section "3D circumferential milling taking into account a limitation surface

(CUT3DCC, CUT3DCCD) (Page 426)".

Job Planning

420

Programming Manual, 12/2018, A5E40869460B AB

Tool offsets

11.5 3D tool radius compensation

Advanced Surface / Top Surface

Note

When applying tool radius compensation CUT3DCD in combination with the "Advanced

Surface" or "Top Surface" option (requiring a license), the setting recommendations regarding

"Advanced Surface" / "Top Surface" must be observed.

Special test programs are provided in the SIOS portal for checking the set data:

● Test programs for Advanced Surface (https://support.industry.siemens.com/cs/ww/en/view/

78956392)

● Test programs for Top Surface (https://support.industry.siemens.com/cs/ww/en/view/

109738423)

11.5.2

Selecting 3D tool radius compensation for the 3D face milling (CUT3DF,

CUT3DFS, CUT3DFF, CUT3DFD)

The 3D tool radius compensation (3D TRC) for the 3D face milling is selected with the modally

effective G command CUT3DF, CUT3DFS, CUT3DFF or CUT3DFD.

The actual activation is performed with G41 or G42

With 3D face milling, the surface normals of the plane to be machined must be defined in order

to calculate the tool radius compensation. This must be performed in the block with G41 or

G42 via the A4, B4, C4 and A5, B5, C5 addresses.

The tool radius compensation is deactivated with G40.

Syntax

G41/G42 ORIC/ORID CUT3DF/CUT3DFS/CUT3DFF/CUT3DFD X... Y... Z... A4=... B4=...

C4=... A5=... B5=... C5=

G40 X... Y... Z...

Meaning

CUT3DFS:

3D TRC for face milling with constant orientation. The tool

orientation is defined by G17 - G19 and is not influenced by

frames.

CUT3DFF:

3D TRC for face milling with constant orientation. The tool

orientation is the direction defined by G17 - G19 and, in some

case, rotated by a frame.

CUT3DF:

3D TRC for face milling with orientation change (only with

active 5-axes transformation)

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

421

Tool offsets

11.5 3D tool radius compensation

CUT3DFD:

3D TRC for face milling with orientation change referred to a

differential tool (only with active 5-axis transformation)

The radius difference is specified by the tool parameter

$TC_DP15.

Note:

CUT3DFD is only possible in combination with "Smoothing

of surface normals in 3D face milling". This is activated by

calling the "Top Surface" function (requires as license) via

CYCLE832(...) (Page 778).

G41/G42 X... Y... Z... :

Activate tool offset

The behavior with G41 and with G42 is identical for 3D face

milling.

Note:

The activation must be performed in a linear block (G0/G1).

A4/5=... B4/5=... C4/5=...:

Definition of the surface normals of the plane to be machined

A4=... B4=... C4=...:

Definition at start of block

A5=... B5=... C5=...:

Definition at end of block

ORIC/ORID:

The behavior for orientation changes at outside corners is

specified via the G commands ORIC and ORID.

ORIC:

Orientation changes at outside corners are su-

perimposed on the circle block to be inserted.

ORID:

Orientation changes are performed before the

circle block.

G40 X... Y... Z... :

Deactivate tool radius compensation

Note:

The deactivation must be performed in a linear block (G0/G1)

with geometry axis movements.

Note

G41 or G42 can also be programmed in blocks without traversing movement in geometry axes

relevant for the compensation. In this case, the approach block is the first traversing block

following such a block.

A change of the 3D TRC variant with active tool radius compensation is ignored without alarm.

Examples

Example 1: 3D face milling with CUT3DF

Program code

Comment

N10

; Definition of tool D1:

N20 $TC_DP1[1,1]=121

; Tool type (toroidal miller)

N30 $TC_DP3[1,1]=20

; Length compensation

N40 $TC_DP6[1,1]=5

; Radius

N50 $TC_DP7[1,1]=3

; Rounding radius

N60

N70

Job Planning

422

Programming Manual, 12/2018, A5E40869460B AB

Tool offsets

11.5 3D tool radius compensation

Program code

Comment

N23 X-248.07130 Y30.15119 Z8.71082

A5=-.060165696 B5=.971048883 C5=-.231179920

A3=-.214177198 B3=.926684940 C3=-.308841625

N24 X-248.07829 Y29.97126 Z8.05094

A5=-.059884286 B5=.968941717 C5=-.239928784

A3=-.213318480 B3=.923853466 C3=-.317789237

N25 X-248.08317 Y29.78487 Z7.38844

A5=-.059584206 B5=.966718449 C5=-.248807482

A3=-.212397895 B3=.920898045 C3=-.326854594

N26 X-248.08578 Y29.59254 Z6.72679

A5=-.059263963 B5=.964380907 C5=-.257793037

A3=-.211418355 B3=.917822366 C3=-.336012474

Note

For 3D face milling with CUT3DFD, the definition of the surface normal is required for activating

the tool offset with G41/G42. Programming of G41/G42 without definition of the surface

normals leads to the output of an alarm.

Further information

3D face milling

For this type of 3D milling, you require the line-by-line description of the 3D paths on the

workpiece surface. The tool shape and dimensions are taken into account in the calculations,

which are normally performed in CAM. The postprocessor writes to the part program - in

addition to NC blocks - the tool orientations (for active 5-axis transformation) and the G

command for the required 3D tool offset. This means that the machine operator has the

possibility of using tools that are slightly smaller - deviating from the tool used to calculate the

NC paths.

Figure 11-3

Face milling

Approach behavior

The approach behavior is always NORM for the 3D variant of the tool radius compensation.

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

425

Tool offsets

11.5 3D tool radius compensation

CUT3DCCD takes account of a limitation surface for a real differential tool that the programmed

standard tool would define. The NC program defines the center-point path of a standard tool.

CUT3DCC with the use of cylindrical tools takes account of a limitation surface that the

programmed standard tool would have reached. The NC program defines the contour on the

machining surface.

The surface normal vector of the limitation surface is specified with A4, B4, C4 and A5, B5,

C5 for 3D face milling.

Syntax

G41/G42 CUT3DCCD/CUT3DCC CDOF2 X... Y... Z... A4=... B4=... C4=... A5=... B5=...

C5=

G40 X... Y... Z...

Meaning

CUT3DCCD:

3D TRC for the circumferential milling taking into account a limitation

surface with a differential tool on the tool center-point path: Infeed

to the limitation surface

CUT3DCC:

3D TRC for the circumferential milling taking into account a limitation

surface with 3D radius compensation: Contour on the machining

surface

G41/G42 X... Y... Z... :

Activate tool radius compensation

G41:

Tool radius compensation left of the contour

G42:

Tool radius compensation right of the contour

Note:

The activation must be performed in a linear block (G0/G1).

CDOF2:

Deactivate collision detection for 3D circumferential milling

A4/5=... B4/5=...

Definition of the surface normals of the limitation surface

C4/5=...:

A4=... B4=... C4=...:

Definition at start of block

A5=... B5=... C5=...:

Definition at end of block

G40 X... Y... Z... :

Deactivate tool radius compensation

Note:

The deactivation must be performed in a linear block (G0/G1) with

geometry axis movements.

Note

The G commands for selecting the 3D TRC are evaluated in the approach block, i.e. typically

in the block that contains G41 or G42.

G41 or G42 can also be programmed in blocks without traversing movement in geometry axes

relevant for the compensation. In this case, the approach block is the first traversing block

following such a block.

A change of the 3D TRC variant with active tool radius compensation is ignored without alarm.

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

427

Tool offsets

11.5 3D tool radius compensation

Example: Toroidal miller with reduced radius compared to the standard tool

Tool type

Shaft radius (R)

Corner radius (r)

Standard tool with corner rounding

R = $TC_DP6

r = $TC_DP7

Real tool with corner rounding

R' = $TC_DP6 + $TC_DP15 +

r' = $TC_DP7 + $TC_DP16

OFFN

Tool types 121 and 131 toroidal

miller

(end mill with corner rounding)

In this example, both $TC_DP15 + OFFN and $TC_DP16 are negative.

3D TRC with CUT3DCCD: Tool center-point path with infeed up to the limitation surface

If a tool with a smaller radius than the appropriate standard tool is used, machining is continued

using a milling tool, which is fed in in the longitudinal direction until it reaches the bottom (base)

of the pocket. The tool removes as much material from the corner formed by the machining

surface and limitation surface. This involves a machining type combining circumferential and

face milling. Analogous to a tool with reduced radius, for a tool with increased radius, the infeed

is in the opposite direction.

① Standard tool

② Tool with smaller radius infeed up to the limitation surface

③ Limitation surface

④ Machining surface

Contrary to all other tool offsets of G group 22, tool parameter $TC_DP6 specified for

CUT3DCCD has no relevance for the tool radius and does not influence the resulting

compensation. The compensation offset results from the sum of the wear value of the tool

radius (tool parameter $TC_DP15) and a tool offset OFFN programmed to calculate the

perpendicular offset to the limitation surface.

The generated part program does not specify whether the surface to be machined is to the

right or left of the path. It is therefore assumed that the radius is a positive value and the wear

value of the original tool is a negative value. A negative wear value always describes a tool

with a reduced diameter.

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

429

Tool offsets

11.5 3D tool radius compensation

Using cylindrical tools

When cylindrical tools are used, infeed is only necessary if the machining surface and the

surface of limitation form an acute angle (less than 90 degrees). If a toroidal miller (end mill

with corner rounding) is used, tool infeed in the longitudinal direction is required for both acute

and obtuse angles.

3D TRC with CUT3DCC: Contour on the machining surface

If CUT3DCC is active with a toroidal miller, the programmed path refers to a fictitious cylindrical

milling tool having the same diameter. The resulting path reference point is shown in the

following diagram for a toroidal miller.

5

① Toroidal miller

② Limitation surface

③ Path reference point

④ Machining surface

R

Shaft radius (tool radius)

The angle between the machining and limitation surfaces may change from an acute to an

obtuse angle and vice versa even within the same block.

The tool actually being used may either be larger or smaller than the standard tool. However,

the resulting corner radius must not be negative and the sign of the resulting tool radius must

be kept.

For CUT3DCC, the NC part program refers to the contour on the machining surface. As for

conventional tool radius compensation, the total tool radius is used that comprises the following

components:

● Tool radius (tool parameter $TC_DP6)

● Wear value (tool parameter $TC_DP15)

● A tool offset OFFN programmed to calculate the perpendicular offset to the limitation surface

The position of the limitation surface is defined from the following difference:

Dimensions of the standard tool - tool radius (tool parameter $TC_DP6)

Job Planning

430

Programming Manual, 12/2018, A5E40869460B AB

Tool offsets

11.6 Tool orientation (ORIC, ORID, OSOF, OSC, OSS, OSSE, ORIS, OSD, OST)

11.6

Tool orientation (ORIC, ORID, OSOF, OSC, OSS, OSSE, ORIS,

OSD, OST)

The term tool orientation describes the geometric alignment of the tool in space. The tool

orientation on a 5-axis machine tool can be set by means of program commands.

=

'LUHFWLRQ YHFWRU

;

<

Orientation rounding movements activated with OSD and OST are formed differently depending

on the type of interpolation for tool orientation.

If vector interpolation is active, the smoothed orientation characteristic is also interpolated

using vector interpolation. On the other hand, if rotary axis interpolation is active, the orientation

is smoothed directly using rotary axis movements.

Programming

Programming a orientation change:

A change in tool orientation can be programmed by:

● Direct programming of rotary axes A, B, C (rotary axis interpolation)

● Euler or RPY angle

● Direction vector (vector interpolation by specifying A3 or B3 or C3)

● LEAD/TILT (face milling)

The reference coordinate system is either the machine coordinate system (ORIMKS) or the

current workpiece coordinate system (ORIWKS).

Job Planning

432

Programming Manual, 12/2018, A5E40869460B AB

Tool offsets

11.6 Tool orientation (ORIC, ORID, OSOF, OSC, OSS, OSSE, ORIS, OSD, OST)

2ULHQWDWLRQ

FKDQJH

Programming tool orientation:

ORIC:

Orientation and path movement in parallel

ORID:

Orientation and path movement consecutively

OSOF:

No orientation smoothing

OSC:

Orientation constantly

OSS:

Orientation smoothing only at beginning of block

OSSE:

Orientation smoothing at beginning and end of block

ORIS:

Velocity of the orientation change with orientation smoothing activated in degrees per

mm (valid for OSS and OSSE)

OSD:

Smoothing of orientation by specifying smoothing distance with setting data:

SD42674 $SC_ORI_SMOOTH_DIST

OST:

Smoothing of orientation by specifying angular tolerance in degrees for vector interpo-

lation with setting data:

SD42676 $SC_ORI_SMOOTH_TOL

With rotary axis interpolation, the specified tolerance is assumed to be the maximum

variance of the orientation axes.

Note

All commands for smoothing the tool orientation (OSOF, OSC, OSS, OSSE, OSD, and OST) are

summarized in G group 34. They are modal; in other words, only one of these commands can

ever be effective at the same time.

Examples

Example 1: ORIC

If two or more blocks with orientation changes are programmed between the traversing blocks

N10 and N20 (e.g. A2=... B2=... C2=...) programmed and ORIC is active, then the

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

433

Tool offsets

11.6 Tool orientation (ORIC, ORID, OSOF, OSC, OSS, OSSE, ORIS, OSD, OST)

inserted circle block is distributed among these intermediate blocks according to the absolute

changes in angle.

1

1

1

1

Program code

Comment

ORIC

N8 A2=… B2=… C2=…

N10 X… Y… Z…

N12 C2=… B2=…

; The circle block inserted at the external corner is

distributed between N12 and N14, corresponding to the

N14 C2=… B2=…

change in orientation. The circular motion and the

orientation change are executed in parallel.

N20 X =…Y=… Z=… G1 F200

Example 2: ORID

If ORID is active, then all blocks between the two traversing blocks are executed at the end of

the first traversing block. The circle block with constant orientation is executed immediately

before the second traversing block.

Job Planning

434

Programming Manual, 12/2018, A5E40869460B AB

Tool offsets

11.6 Tool orientation (ORIC, ORID, OSOF, OSC, OSS, OSSE, ORIS, OSD, OST)

3HUIRUP 1 DQG 1

1

1

Program code

Comment

ORID

N8 A2=… B2=… C2=…

N10 X… Y… Z…

N12 A2=… B2=… C2=…

; The N12 and N14 blocks are executed at the end of N10.

The circle block is then executed with the actual orien-

tation.

N14 M20

; Help functions, etc.

N20 X… Y… Z…

Note

The method which is used to change orientation at an outer contour is determined using the

program command that is active in the first traversing block of an outer corner.

Without change in orientation: If the orientation is not changed at the block boundary, the cross-

section of the tool is a circle, which touches both of the contours.

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

435

Tool offsets

11.6 Tool orientation (ORIC, ORID, OSOF, OSC, OSS, OSSE, ORIS, OSD, OST)

Example 3: Change in orientation at an inside corner

1

1

1

:5.

Program code

ORIC

N10 X …Y… Z… G1 F500

N12 X …Y… Z… A2=… B2=… C2=…

N15 X …Y… Z… A2=… B2=… C2=…

Further information

Behavior at outer corners

A circle block with the radius of the cutter is always inserted at an outside corner.

The ORIC and ORID program commands are used to determine whether changes in orientation

programmed between block N1 and N2 are executed before the inserted circle block is

processed or at the same time.

Job Planning

436

Programming Manual, 12/2018, A5E40869460B AB

Tool offsets

11.6 Tool orientation (ORIC, ORID, OSOF, OSC, OSS, OSSE, ORIS, OSD, OST)

$ FLUFXODU EORFN ZLOO EH DGGHG

EHWZHHQ EORFN 1 DQG 1

1

1

5

If an orientation change is required at outside corners, this can be performed either at the same

time as interpolation or separately together with the path movement.

When ORID is programmed, the inserted blocks are executed first without path motion. The

circle block generating the corner is inserted immediately before the second of the two

traversing blocks.

If several orientation blocks are inserted at an external corner and ORIC is selected, the circular

motion is distributed among the individual inserted blocks according to the absolute values of

the orientation changes.

Smoothing orientation with OSD or OST

When blending with G642, the maximum variance for the contour axes and orientation axes

cannot vary greatly. The smaller tolerance of the two determines the type of smoothing motion

and/or angular tolerance to smooth the orientation characteristic relatively strongly without

having to accept higher contour deviations.

OSD and OST can be activated to "generously" smooth very slight deviations from the

orientation characteristics with a specified smoothing distance and angular tolerance without

serious contour deviations.

Note

Unlike the process of rounding the contour (and orientation characteristics) with G642, when

rounding the orientation with OSD and/or OST, a separate block is not formed, instead the

rounding movement is added directly to the programmed original blocks.

With OSD and/or OST, block transitions cannot be rounded if there is a change in the type of

interpolation for tool orientation (vector → rotary axis, rotary axis → vector). These block

transitions can if necessary be rounded with the standard rounding functions G641, G642 and

G643.

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

437

Tool offsets

11.7 Free assignment of D numbers, cutting edge numbers

11.7

Free assignment of D numbers, cutting edge numbers

11.7.1

Free assignment of D numbers, cutting edge numbers (CE address)

D number

The D numbers can be used as offset numbers. The number of the cutting edge can also be

addressed via the CE address. The cutting edge number can be written by the system variable

$TC_DPCE.

Default setting: Compensation no. == cutting edge no.

Machine data are used to define the maximum number of D numbers (cutting edge numbers)

and the maximum number of cutting edges per tool (→ machine manufacturer). The following

commands are only practical if the maximum cutting edge number (MD18105) was specified

to be greater than the number of cutting edges per tool (MD18106). Observe the machine

manufacturer’s specifications.

References

Function Manual Basic Functions; Tool Offset (W1)

11.7.2

Free assignment of D numbers: Checking D numbers (CHKDNO)

Using the CKKDNO command, you can check whether the existing D numbers were uniquely

assigned. The D numbers of all tools defined within a TO unit may not occur more than once.

No allowance is made for replacement tools.

Syntax

state=CHKDNO(Tno1,Tno2,Dno)

Meaning

state:

=TRUE:

The D numbers are assigned uniquely to the checked

areas.

= FALSE:

There was a D number collision or the parameters are

invalid. Tno1, Tno2 and Dno return the parameters

that caused the collision. These data can now be eval-

uated in the part program.

CHKDNO(Tno1,Tno2):

All D numbers of the part specified are checked.

CHKDNO(Tno1):

All D numbers of Tno1 are checked against all other tools.

CHKDNO:

All D numbers of all tools are checked against all other tools.

Job Planning

438

Programming Manual, 12/2018, A5E40869460B AB

Tool offsets

11.7 Free assignment of D numbers, cutting edge numbers

11.7.3

Free assignment of D numbers: Rename D numbers (GETDNO, SETDNO)

You must assign unique D numbers. Two different cutting edges of a tool must not have the

same D number.

GETDNO

This command returns the D number of a particular cutting edge (ce) of a tool with tool number

t. If no D number exists for the entered parameters, d=0 will be set. If the D number is invalid,

a value greater than 32000 is returned.

SETDNO

This command assigns the value d of the D number to a cutting edge (ce) of tool t. The result

of this statement is returned via state (TRUE or FALSE). If there is no data block for the

specified parameter, the value FALSE is returned. Syntax errors generate an alarm. The D

number cannot be set explicitly to 0.

Syntax

d = GETDNO (t,ce)

state = SETDNO (t,ce,d)

Meaning

d:

D number of the tool edge

t:

T number of the tool

ce:

Cutting edge number (CE number) of the tool

state:

Indicates whether the command could be executed (TRUE or FALSE).

Example for renaming a D number

Programming

Comment

$TC_DP2[1.2]=120

$TC_DP3[1,2]

= 5.5

$TC_DPCE[1,2] = 3

; Cutting edge number CE

N10 def int DNoOld, DNoNew = 17

N20 DNoOld = GETDNO(1,3)

N30 SETDNO(1,3,DNoNew)

The new D value 17 is then assigned to cutting edge CE=3. Now the data for the cutting edge

is addressed via D number 17; both via the system variables and in the programming with the

NC address.

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

439

Tool offsets

11.7 Free assignment of D numbers, cutting edge numbers

11.7.4

Free assignment of D numbers: Determine T number to the specified D number

(GETACTTD)

The pre-defined function GETACTTD determines the T number associated with an absolute

D number. There is no check for uniqueness. If several D numbers within a TO unit are the

same, the T number of the first tool found in the search is returned.

Syntax

<Status>=GETACTTD(<TNo>,<DNo>)

Meaning

GETACTTD():

Function call

<DNo>:

D number for which the T number shall be searched.

Data type:

INT

<TNo>:

T number found

Data type:

VAR INT

<status>:

Result

Data type:

INT

Value:

0

The T number was found. <Tno> contains the value of the T

number.

-1

No T number exists for the specified D number; <Tno>=0.

-2

The D number is not absolute. <TNo> receives the value of

the first tool found that contains the D number with the value

<Dno>.

-5

The function was not able to be executed for another reason.

11.7.5

Free assignment of D numbers: Invalidate D numbers (DZERO)

The DZERO command is used for support during retooling. Compensation data sets tagged

with this command are no longer verified by the CHKDNO command. These data sets can be

accessed again by setting the D number once more with SETDNO.

Syntax

DZERO

Meaning

DZERO:

Marks all D numbers of the TO unit as invalid.

Job Planning

440

Programming Manual, 12/2018, A5E40869460B AB

Tool offsets

11.8 Toolholder kinematics

11.8

Toolholder kinematics

Requirements

A toolholder can only orientate a tool in all possible directions in space if

● Two rotary axes V₁ and V₂ are present.

● The rotary axes are mutually orthogonal.

● The tool longitudinal axis is perpendicular to the second rotary axis V₂.

In addition, the following requirement is applicable to machines for which all possible

orientations have to be settable:

● The tool longitudinal axis must be perpendicular to the first rotary axis V₁.

Function

The toolholder kinematics with a maximum of two rotary axes v₁ or v₂ are defined using the 17

system variables $TC_CARR1[m] to $TC_CARR17[m]. The description of the toolholder

consists of:

● The vectoral distance from the first rotary axis of the toolholder I₁, the vectoral distance

from the first rotary axis to the second rotary axis I₂, the vectoral distance from the second

rotary axis to the reference point of the tool I₃.

● The direction vectors of both rotary axes V₁, V₂.

● The angles of rotation α1, α2 around the two axes. The rotation angles are counted in

viewing direction of the rotary axis vectors, positive, in clockwise direction of rotation.

O

9

˞

O

O

˞

9

For machines with resolved kinematics (both the tool and the part can rotate), the system

variables have been extended with the entries $TC_CARR18[m] to $TC_CARR23[m].

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

441

Tool offsets

11.8 Toolholder kinematics

Parameters

Function of the system variables for orientable toolholders

Designation

x component

y component

z component

l₁ offset vector

$TC_CARR1[m]

$TC_CARR2[m]

$TC_CARR3[m]

l₂ offset vector

$TC_CARR4[m]

$TC_CARR5[m]

$TC_CARR6[m]

v₁ rotary axis

$TC_CARR7[m]

$TC_CARR8[m]

$TC_CARR9[m]

v₂ rotary axis

$TC_CARR10[m]

$TC_CARR11[m]

$TC_CARR12[m]

α₁ angle of rota-

$TC_CARR13[m]

tion

$TC_CARR14[m]

α₂ angle of rota-

tion

l₃ offset vector

$TC_CARR15[m]

$TC_CARR16[m]

$TC_CARR17[m]

Extensions of the system variables for orientable toolholders

Designation

x component

y component

z component

l₄ offset vector

$TC_CARR18[m]

$TC_CARR19[m]

$TC_CARR20[m]

Axis identifier Ro-

Axis identifier of the rotary axes v₁ and v₂ (initialized with zero)

tary axis v₁

$TC_CARR21[m]

Rotary axis v₂

$TC_CARR22[m]

Kinematic type

$TC_CARR23[m]

Tool

Kinematics type T ->

Kinematics type P ->

Kinematics type M

Part

Only the tool can rotate

Only the part can rotate

Part and tool can rotate

Mixed mode

(default).

Offset of the

Angle in degrees of the rotary axes v₁ and v₂ on assuming the initial setting

Rotary axis v₁

$TC_CARR24[m]

Rotary axis v₂

$TC_CARR25[m]

Angle offset of

Offset of the Hirth tooth system in degrees for rotary axes v₁ and v₂

the rotary axis v₁

$TC_CARR26[m]

Rotary axis v₂

$TC_CARR27[m]

Angle increment

Offset of the Hirth tooth system in degrees for rotary axes v₁ and v₂

v₁ rotary axis

$TC_CARR28[m]

v₂ rotary axis

$TC_CARR29[m]

Min. position Ro-

Software limit for the minimum position of the rotary axes v₁ and v₂

tary axis v₁

$TC_CARR30[m]

Rotary axis v₂

$TC_CARR31[m]

Max. position Ro-

Software limits for the maximum position of the rotary axes v₁ and v₂

tary axis v₁

$TC_CARR32[m]

Rotary axis v₂

$TC_CARR33[m]

Toolholder name

A toolholder can be given a name instead of a number. $TC_CARR34[m]

User:

Intended use in user measuring cycles $TC_CARR35[m]

Axis name 1

$TC_CARR36[m]

Axis name 2

$TC_CARR37[m]

Identifier

$TC_CARR38[m]

$TC_CARR39[m]

$TC_CARR40[m]

Position

Fine

Parameters that can be added to the values

offset

in the basic parameters.

l₁ offset vector

$TC_CARR41[m]

$TC_CARR42[m]

$TC_CARR43[m]

Job Planning

442

Programming Manual, 12/2018, A5E40869460B AB

Tool offsets

11.8 Toolholder kinematics

Extensions of the system variables for orientable toolholders

l₂ offset vector

$TC_CARR44[m]

$TC_CARR45[m]

$TC_CARR46[m]

l₃ offset vector

$TC_CARR55[m]

$TC_CARR56[m]

$TC_CARR57[m]

l₄ offset vector

$TC_CARR58[m]

$TC_CARR59[m]

$TC_CARR60[m]

v₁ rotary axis

$TC_CARR64[m]

v₂ rotary axis

$TC_CARR65[m]

Note

Explanations of parameters

"m" specifies the number of the toolholder to be programmed.

$TC_CARR47 to $TC_CARR54 and $TC_CARR61 to $TC_CARR63 are not defined and

produce an alarm if read or write access is attempted.

The start/end points of the distance vectors on the axes can be freely selected. The rotation

angles α₁, α₂ around the two axes are defined in the initial state of the toolholder by 0°. In this

way, the kinematics of a toolholder can be programmed for any number of possibilities.

Toolholders with only one or no rotary axis at all can be described by setting the direction

vectors of one or both rotary axes to zero.

With a toolholder without rotary axis the distance vectors act as additional tool offsets whose

components cannot be affected by a change of machining plane (G17 to G19).

Parameter extensions

Parameters of the rotary axes

The system variables have been extended by the entries $TC_CARR24[m] to

$TC_CARR33[m] and described as follows:

Offset of rotary axes

Changing the position of the rotary axis v₁ or v₂ for the initial setting of the ori-

v₁, v₂

ented toolholder.

The angle offset/an-

The offset or the angle increment of the Hirth tooth system of the rotary axes

gle increment of the

v₁ and v₂. Programmed or calculated angle is rounded up to the next value that

rotary axes v₁, v₂

results from phi = s + n * d when n is an integer.

The minimum and

The minimum and maximum position of the rotary axis limit angle (software limit)

maximum position of

of the rotary axes v1 and v2.

the rotary axes v₁, v₂

Parameters for the user

$TC_CARR34 to $TC_CARR40 contain parameters that are freely available to users and up

to SW 6.4 were as standard, not further evaluated within the NCK or had no significance.

Fine offset parameters

$TC_CARR41 to $TC_CARR65 include fine offset parameters that can be added to the values

in the basis parameters. The fine offset value assigned to a basic parameter is obtained when

the value 40 is added to the parameter number.

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

443

Tool offsets

11.8 Toolholder kinematics

Example

The toolholder used in the following example can be fully described by a rotation around the

Y axis.

]

]

=

<

<

=

;

<

;

;

;

Program code

Comment

N10 $TC_CARR8[1]=1

; Definition of the Y component of

the first rotary axis of toolholder

1.

N20 $TC_DP1[1,1] = 120

; Definition of a shaft miller.

N30 $TC_DP3[1,1]=20

; Definition of a shaft miller, 20

mm long.

N40 $TC_DP6[1,1]=5

; Definition of a shaft miller with

5 mm radius.

N50 ROT Y37

; Frame definition with 37° rota-

tion around the Y axis.

N60 X0 Y0 Z0 F10000

; Approach start position.

N70 G42 CUT2DF TCOFR TCARR=1 T1 D1 X10

Set radius compensation, tool

length compensation in rotated

frame, select toolholder 1, tool 1.

N80 X40

; Perform machining under a rota-

tion of 37°.

N90 Y40

N100 X0

N110 Y0

N120 M30

Job Planning

444

Programming Manual, 12/2018, A5E40869460B AB

Tool offsets

11.9 Tool length compensation for orientable toolholders (TCARR, TCOABS, TCOFR, TCOFRX, TCOFRY,

TCOFRZ)

11.9

Tool length compensation for orientable toolholders (TCARR,

TCOABS, TCOFR, TCOFRX, TCOFRY, TCOFRZ)

When the spatial orientation of the tool changes, its tool length components also change.

=

=

,

,

,

;

;

After a reset, e.g. through manual setting or change of the toolholder with a fixed spatial

orientation, the tool length components also have to be determined again. This is performed

using the TCOABS and TCOFR path commands.

For a toolholder of an active frame that can be orientated, when selecting the tool with TCOFRZ,

TCOFRY and TCOFRX, it is possible to define the direction in which the tool should point.

Syntax

TCARR=[<m>]

TCOABS

TCOFR

TCOFRZ

TCOFRY

TCOFRX

Meaning

TCARR=[<m>]:

Request toolholder with the number "m"

TCOABS:

Determine tool length components from the orientation of the current toolholder

TCOFR:

Determine tool length components from the orientation of the active frame

TCOFRZ:

Orientable toolholder from active frame with a tool pointing in the Z direction

TCOFRY:

Orientable toolholder from active frame with a tool pointing in the Y direction

TCOFRX:

Orientable toolholder from active frame with a tool pointing in the X direction

Job Planning

446

Programming Manual, 12/2018, A5E40869460B AB

Tool offsets

11.10 Online tool length compensation (TOFFON, TOFFOF)

11.10

Online tool length compensation (TOFFON, TOFFOF)

Use the system variable $AA_TOFF[<n> ] to overlay the effective tool lengths in accordance

with the three tool directions three-dimensionally in real time.

The three geometry axis identifiers are used as index <n>. Thus, the number of active direction

offsets is determined by the geometry axes that are active at the same time.

All offsets can be active at the same time.

The online tool length offset function can be used for:

● Orientation transformation TRAORI

● Orientable toolholder TCARR

Note

Online tool length offset is an option, which must be enabled in advance. This function is

only practical in conjunction with an active orientation transformation or an active orientable

toolholder.

Syntax

TRAORI

TOFFON(<compensation direction>[,<offset value>])

WHEN TRUE DO $AA_TOFF[<compensation direction>]

; In synchronized actions.

TOFFOF(<compensation direction>)

For more information about programming online tool length offset in motion-synchronous

actions, see "Synchronized actions (Page 597)".

Meaning

TOFFON:

Activate online tool length offset

<compensation

Tool direction (X, Y, Z), in which the online tool length

direction>:

offset should be active.

<offset value>:

When activating, an offset value can be specified for

the relevant direction of compensation and this is im-

mediately recovered.

TOFFOF:

Reset online tool length offset

The compensation values in the specified compensation direction are reset and a pre-

processing stop is initiated.

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

449

Tool offsets

11.11 Modification of the offset data for rotatable tools

Meaning

ORISOLH:

Function call

<RetVal>:

Function return value

Data type:

INT

Range of val-

0, -2, -3, ..., -17

ues:

Values:

0

Function has ended without an error.

-2

No valid transformation (6-axis orientation transformation) is

active.

-3

The first parameter (<Cntrl>) is negative.

-4

The unit position of the first parameter (<Cntrl>) is invalid.

Only the values 0 and 1 are permissible.

-5

The tens position of the first parameter (<Cntrl>) is invalid.

Only the values 0 to 3 are permissible.

-6

The hundreds position of the first parameter (<Cntrl>) is in-

valid.

Only the values 0 and 1 are permissible.

-7

The thousands position of the first parameter (<Cntrl>) is in-

valid.

Only the values 0 to 3 are permissible.

-8

Angle γ is too large for the "Direct tool alignment" function.

-9

At least one of the specified axis positions violates an axis

limit for the "Direct tool alignment" function.

-10

No tool is active.

-11

The requested orientation cannot be set.

-12

The adaptation of the free axis angle for the Hirth joint is not

possible for the first or only solution.

-13

The adaptation of the free axis angle for the Hirth joint is not

possible for the second solution.

-14

The adaptation of the free axis angle for the Hirth joint is not

possible for either of the two solutions.

-15

The first orientation axis is parameterized as Hirth axis.

-16

The second as well as the third rotary axis has been para-

meterized as Hirth axis. Only one of the two axes can be the

Hirth axis.

-17

At least one of the specified axis positions is not compatible

with the associated Hirth joint for the "Swivel directly" func-

tion.

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

453

Tool offsets

11.11 Modification of the offset data for rotatable tools

<Cntrl>:

Controls the behavior of the function

Data type:

INT

The <Cntrl> parameter is decimal coded (unit to thousands position):

Unit position:

The unit position controls the response to errors.

xxx0

In the event of an error (return value < 0), alarm 14106 is

output and program processing is aborted.

Note:

The alarm is also output irrespective of the value of the unit

position when the <Cntrl> parameter is negative.

xxx1

In the event of an error (return value < 0) no alarm is output.

The user can react suitably in the program.

Tens position:

Controls the behavior when an orientation axis with Hirth joint is

present.

Note:

This parameter is only evaluated for the "Tool alignment" function

(i.e. when the hundreds position has the value "0").

xx0x

The axis position is rounded off to the nearest position.

xx1x

The axis positions are rounded off so that the difference of

the β angle to its programmed value is minimal.

xx2x

The axis positions are rounded off so that the β angle is equal

to the highest possible value which is less than the program-

med value (β is rounded down).

xx3x

The axis positions are rounded off so that the β angle is equal

to the lowest possible value which is greater than the pro-

grammed value (β is rounded up).

Hundreds posi-

Specifies which function is to be executed or the significance of the

tion:

two following parameters <W1> and <W2>.

x0xx

"Tool alignment" function

Parameters <W1> and <W2> have the following meaning:

● <W1> = β

● <W2> = γ

The associated angles of the orientation axes are calculated.

x1xx

"Direct tool alignment" function

<W1> is the position specification for the second orientation

axis, <W2> is the position specification for the third orienta-

tion axis of a 6-axis transformation. The position of the first

orientation axis and the β and γ angles are defined which are

compatible with the two position specifications.

If no error occurs, two solutions are always output in the

$P_ORI_POS[<n>, <m>] system variables. The first index

<n> (0 or 1) refers to the solution and the second index <m>

(0 ... 2) to the orientation axis:

● $P_ORI_POS[0/1, 0]: Position of the first orientation axis

● $P_ORI_POS[0/1, 1]: Angle β

● $P_ORI_POS[0/1, 2]: Angle γ

A check is made as to whether the position specifications

<W1> and <W2> are compatible with any Hirth joints or active

software limits. If this is not the case, a corresponding error

number is returned (see <RetVal> parameter).

Job Planning

454

Programming Manual, 12/2018, A5E40869460B AB

Tool offsets

11.11 Modification of the offset data for rotatable tools

If the angles <W1> and <W2> are selected arbitrarily, the

cutting edge of the tool is generally not in the machining

plane. The angle γ through which the cutting edge is rotated

out of the machining plane, must not be greater than the limit

value which is defined by the setting data SD42999 $SC_OR-

ISOLH_INCLINE_TOL.

Thousands po-

Specifies which positions of the solutions may be modified when the

sition:

hundreds position has the value "0", i.e. for the "Tool alignment"

function.

0xxx

The calculated axis positions should be as close as possible

to the current machine axis positions.

1xxx

The calculated axis positions for modulo axes should be as

close as possible to the middle of the modulo range, for other

axes as close as possible to 0. For non-modulo axes, this

means that the axis positions are reduced to the range

-180° … +180°.

2xxx

The calculated axis positions should be reduced to the range

-180° … +180° irrespective of the axis type.

<W1>:

First angle

The meaning results from the hundreds position of the <Cntrl> paramter.

Data type:

REAL

<W1>:

Second angle

The meaning results from the hundreds position of the <Cntrl> paramter.

Data type:

REAL

Note

Parameters that have not been programmed have the default value "0".

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

455

Tool offsets

11.11 Modification of the offset data for rotatable tools

Further information

The number of solutions found together with further status information when executing the

ORISOLH function, can be read via the following system variables:

System variable

Meaning

$P_ORI_POS

Returns the angles of the orientation axes that result from the orientation program-

[<n>, <m>]

ming.

<n>:

Index of the solution

Range of values:

0, 1

<m>:

Index of the orientation axis

Range of values:

0 ... 2

The order of the orientation axes (1 ... 3) refers to the

definition of the axes in $NT_ROT_AX_NAME.

When the ORISOLH function is called in the "Direct tool alignment" mode, the

$P_ORI_POS[0/1, 1] and P_ORI_POS[0/1, 2] variables contain the values of the

two angles β and γ belonging to the two solutions.

The first solution entered in $P_ORI_POS[<n>, <m>], i.e. with the index <n> = 0, is

always the solution that is selected by the control when the requested orientation

is approached directly. The second index <m> refers to the orientation axis, i.e. on

$NT_ROT_AX_NAME.

The axis positions entered in $P_ORI_POS[<n>, <m>] take into account the offsets

entered in $NK_OFF and $NK_OFF_FINE, i.e. these axis angles can be used in the

following blocks to set the required orientation without any further modification.

If a rotary axis is a Hirth axis, the solution positions are rounded off to the nearest

position of rest of the Hirth joint. For Hirth jointed rotary axes, you can read the

differences between the axis positions for the exact solutions and those of the sol-

utions adapted to the Hirth incrementing in the $P_ORI_DIFF system variable.

$P_ORI_DIFF

Returns the difference between the exact positions of the orientation axes and those

[<n>, <m>]

provided in $P_ORI_POS that result from the orientation programming.

<n>:

Index of the solution

Range of values:

0, 1

<m>:

Index of the orientation axis

Range of values:

0 ... 2

The order of the orientation axes (1 ... 3) refers to the

definition of the axes in $NT_ROT_AX_NAME.

The content can only be not equal to zero when the positions are incremented (Hirth

joint), i.e. when the system data $NT_HIRTH_INCR of the relevant axis is not equal

to zero and when this axis is a manual rotary axis.

Job Planning

456

Programming Manual, 12/2018, A5E40869460B AB

Tool offsets

11.11 Modification of the offset data for rotatable tools

System variable

Meaning

$P_ORI_SOL

If for an orientation transformation with more than one orientation axis, the axis

angles are calculated that should result in a specified orientation, there is generally

more than one solution. The $P_ORI_SOL system variables contain the number of

valid solutions together with additional status information.

The content of $P_ORI_SOL is coded as follows:

Values < 0

General error states

-1

No solutions have been calculated yet for the active transfor-

mation (missing call of ORISOLH).

-2

A transformation is not active, or the active transformation is

not an orientation transformation (6-axis transformation) that

can provide positions for a specified orientation programming.

-4

The desired orientation cannot be set with the present kine-

matics.

-5

No solution was found when the ORISOLH function was called

in the "Direct tool alignment" mode.

-6

Angle γ is too large when the ORISOLH function was called

in the "Direct tool alignment" mode.

-7

An angle was specified when the ORISOLH function was

called in the "Direct tool alignment" mode that cannot be set

because of the Hirth joint.

-8

The first orientation axis (frame axis) must not be parameter-

ized as Hirth axis.

-9

The second as well as the third rotary axis has been parame-

terized as Hirth axis. Only one of the two axes can be the Hirth

axis.

-10

No adaptation of the solution(s) to the Hirth joint has been

found.

Values > 0

Number of mathematically possible solutions without consideration

of axis limits and any error conditions.

Unit position

0

There is no solution, i.e. the requested orientation cannot be

set.

There can be three different causes for this case:

● In principle, the requested orientation cannot be achieved

because of the machine kinematics (orientation axes not

arranged at right angles) even with an arbitrary traversing

range of the orientation axes. In this case, the tens and

hundreds positions of $P_ORI_SOL are both zero, the

$P_ORI_STAT status variables assigned to the orientation

axis have the value "-4".

● The calculated solutions cannot be achieved because they

would violate the axis limits. The positions of the

orientation axes that would result without the axis limits,

can be read in $P_ORI_POS.

● Axis positions were specified when the ORISOLH function

was called in the "Direct tool alignment" mode which would

result in either the orientation vector or the orientation

normal vector of the tool being aligned parallel to the first

orientation axis, whose position is to be calculated. The

position of this axis is not defined in these cases.

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

457

Tool offsets

11.11 Modification of the offset data for rotatable tools

System variable

Meaning

1

There is a solution.

There can be three different causes for this case:

● Based on the specified orientation and the machine

kinematics, there is only one solution (from the

mathematical point of view, two coinciding solutions) even

without consideration of the axis limits. This case occurs

at the edge of the orientation range for kinematics that are

not at right angles. $P_ORI_POS contains both (identical)

solutions.

● There is only one solution because a second solution is

invalid due to the violated axis limits. The valid solution is

always the first solution in $P_ORI_POS. The second

solution which would result when the axis limits are not

taken into account, can also be read in $P_ORI_POS.

● This is the normal case when the ORISOLH function is

called in the "Direct tool alignment" mode. For the specified

axis positions of two orientation axes, there is generally

only one valid position for the missing orientation axis to

be calculated.

2

There are two solutions.

8

There are an infinite number of solutions, i.e. the position of

an orientation axis (the polar axis) is arbitrary. However, from

the two possible positions of the other axes, one is excludes

because of the violated axis limits.

9

There are an infinite number of solutions, i.e. the position of

an orientation axis (the polar axis) is indefinite. The indefinite

axis can be determined from the hundreds position or from the

$P_ORI_STAT system variable.

Values > 0

Bit-coded display for violated axis limits. The precise cause of the

error can be determined from the $P_ORI_STAT system variable.

Tens posi-

tion

Bit 0 (value 10):

For at least one solution, at least one axis limit

of the first orientation axis is violated.

Bit 1 (value 20):

For at least one solution, at least one axis limit

of the second orientation axis is violated.

Bit 2 (value 40):

For at least one solution, at least one axis limit

of the third orientation axis is violated.

Values > 0

Bit-coded display for non-defined axis positions (can only occur when

there is an infinite number of solutions, i.e. when the unit position is

Hundreds

equal to "9").

position

Bit 0 (value 100):

The position of the first orientation axis is not de-

fined.

Bit 1 (value 200):

The position of the second orientation axis is not

defined.

Bit 2 (value 400):

The position of the third orientation axis is not

defined.

The designations first, second and third orientation axis refer to the definition of the

axes in $NT_ROT_AX_NAME.

Job Planning

458

Programming Manual, 12/2018, A5E40869460B AB

Tool offsets

11.11 Modification of the offset data for rotatable tools

System variable

Meaning

$P_ORI_STAT

Returns the status for each of the maximum three orientation axes after ORISOLH

[<n>]

has been called.

<n>:

Index of the orientation axis

(correspnds to the index of the relevant orientation axis in

$NT_ROT_AX_NAME)

Range of values:

0 ... 2

The order of the orientation axes (1 ... 3) refers to the

definition of the axes in $NT_ROT_AX_NAME.

The content of $P_ORI_STAT is coded as follows:

Values < 0

General error states

-1

The status is not defined (missing call of ORISOLH).

-2

A transformation is not active, or the active transformation is

not an orientation transformation (6-axis transformation) that

can provide positions for a specified orientation programming.

-3

The axis is not included in the active transformation.

-4

The position of the axis cannot be calculated because the re-

quested orientation cannot be achieved with the present kin-

ematics even with an arbitrary assumed traversing range of

the axis.

-5

Axis positions were specified when the ORISOLH function

was called in the "Direct tool alignment" mode which would

result in either the orientation vector or the orientation normal

vector of the tool being aligned parallel to the first orientation

axis, whose position is to be calculated. The position of this

axis is not defined in these cases.

-6

Angle γ is too large when the ORISOLH function was called

in the "Direct tool alignment" mode.

-7

An angle was specified when the ORISOLH function was

called in the "Direct tool alignment" mode that cannot be set

because of the Hirth joint.

-8

The first orientation axis (frame axis) must not be parameter-

ized as Hirth axis.

-9

The second as well as the third rotary axis has been parame-

terized as Hirth axis. Only one of the two axes can be the Hirth

axis.

-10

No adaptation of the solution(s) to the Hirth joint has been

found.

Values > 0

Bit-coded display for violated axis limits of the first solution.

Unit position

Bit 0 (value 1):

The first solution violates the lower axis limit.

Bit 1 (value 2):

The first solution violates the upper axis limit.

Values > 0

Bit-coded display for violated axis limits of the second solution.

Tens posi-

Bit 0 (value 10):

The second solution violates the lower axis limit.

tion

Bit 1 (value 20):

The second solution violates the upper axis limit.

Values > 0

Display of a non-defined axis position.

Hundreds

Bit 0 (value 100):

The position of the orientation axis is not defined,

position

i.e. the requested orientation is achieved with

each arbitrary setting of the rotary axis (polar po-

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

459

Tool offsets

11.11 Modification of the offset data for rotatable tools

System variable

Meaning

sition). This information is also contained in the

$P_ORI_SOL system variable.

Of the error numbers that indicate a violation of the axis limits, several can occur

simultaneously. When an axis limit is violated, an attempt is made to reach a position

within the permissible axis limits by adding or subtracting multiples of 360°. If this

is not possible, it is not clearly defined whether the lower or the upper axis limit has

been violated.

If there is no solution for the requested orientation ($P_ORI_SOL = 0), the status of

the orientation axes in the transformation is "0".

Note

$NT_ROT_AX_NAME

This system variable refers to a maximum of three axes used for setting the orientation. It

contains the names of the chain elements ($NK_NAME) that define the machine axes (rotary

axes) that must perform the orientation movements resulting from a kinematic transformation.

The order in which the maximum three rotary axes are contained in this system variable is

irrelevant for the machine kinematics because this is derived from the structure of the kinematic

chains. However, as it defines the order in which other variables access the rotary axes, the

order of the orientation axes in $NT_ROT_AX_NAME must match the kinematic description.

Note

Status information

The status information that shows, for example, that an orientation cannot be achieved or can

only be achieved when relevant axis limits are violated, does not trigger an NC alarm. It is the

responsibility of the user to react suitably to the specified conditions.

11.11.2

Activating the modification of the offset data for rotatable tools (CUTMOD,

CUTMODK)

The modification of the offset data for rotatable tools is activated in the NC program via the

CUTMOD (in combination with orientable tool carriers) or CUTMODK language command (for

orientation transformations that were defined by means of kinematic chains).

Note

As the orientable tool carriers and orientation transformations that were defined by means of

kinematic chains cannot be active at the same time, there are no conflicts between the two

variants.

Syntax

CUTMOD = <Value>

or

Job Planning

460

Programming Manual, 12/2018, A5E40869460B AB

Tool offsets

11.11 Modification of the offset data for rotatable tools

CUTMODK = <Command>

Meaning

CUTMOD:

Function call in combination with orientable tool carriers

<Value>:

Assigned value

Data type:

INT

Value:

0

The function is deactivated.

The values supplied from system variables $P_AD... are the same

as the corresponding tool parameters.

> 0

The function is activated if an orientable tool carrier with the speci-

fied number is active, i.e. the activation is linked to a specific ori-

entable tool carrier.

The values supplied from system variables $P_AD... may be modi-

fied with respect to the corresponding tool parameters depending

on the active rotation.

The deactivation of the designated orientable tool carrier tempo-

rarily deactivates the function; the activation of another orientable

tool carrier permanently deactivates it. This is the reason why in

the first case, the function is re-activated when again selecting the

same orientable tool carrier; in the second case, a new selection

is required - even if at a subsequent time, the orientable tool carrier

is re-activated with the specified number.

The function is not influenced by a reset.

-1

The function is always activated if an orientable tool carrier is ac-

tive.

When changing the tool carrier or when de-selecting it and a sub-

sequent new selection, CUTMOD does not have to be set again.

-2

The function is always activated if an orientable tool carrier is ac-

tive whose number is the same as the currently active orientable

tool carrier.

If an orientable tool carrier is not active, then this has the same

significance as CUTMOD=0.

If an orientable tool carrier is active, then this has the same signif-

icance as when directly specifying the actual tool carrier number.

< -2

Values less than 2 are ignored, i.e. this case is treated as if CUT-

MOD was not programmed.

Note:

This value range should not be used as it is reserved for possible

subsequent expansions.

CUTMODK:

Function call in combination with orientation transformations that have been defined by

means of kinematic chains

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

461

Tool offsets

11.11 Modification of the offset data for rotatable tools

<Command>:

Assigned Command

Data type:

STRING

Value:

"NEW"

The states of an active transformation defined with kinematic

chains relevant for the "Modification of the offset data", the

name of the transformation and the current contour frame

are saved.

Note:

This command is only permissible when a suitable transfor-

mation (TRAORI_DYN, TRAORI_STAT or TRAANG_K) is

active.

"OFF"

Switches the active "Modification of the offset data" off. The

data previously stored with "NEW" is retained.

Note:

This command is also permissible when CUTMODK is not

active. It then remains without effect. Any data set present

for the "Modification of the offset data" is retained.

"ON"

With this command, the "Modification of the offset data" is

re-activated with a data set previously stored with the "NEW"

command.

If a transformation with the name of the stored data set is

active when this command is executed, the "Modification of

the offset data" takes effect immediately. Otherwise, the ac-

tivation is delayed until an active transformation is activated.

"CLEAR"

As with the "OFF" command, switches the "Modification of

the offset data" off and also deletes the stored data set.

Note:

This command is also permissible when CUTMODK is not

active.

Note

SD42984 $SC_CUTDIRMOD

The CUTMOD or CUTMODK command replaces the function that can be activated using the

setting data SD42984 $SC_CUTDIRMOD. However, this function remains available

unchanged. However, as it doesn't make sense to use both functions in parallel, it can only be

activated if CUTMOD is equal to zero and CUTMODK is the zero string.

Further information

Reading modified offset data

The modified offset data is provided in the following system variables and OPI variables:

Meaning

System variable

OPI variable

Cutting edge position

$P_AD[2]

cuttEdgeParam2

Holder angle

$P_AD[10]

cuttEdgeParam10

Cut direction

$P_AD[11]

cuttEdgeParam11

Clearance angle

$P_AD[24]

cuttEdgeParam24

Job Planning

462

Programming Manual, 12/2018, A5E40869460B AB

Tool offsets

11.11 Modification of the offset data for rotatable tools

The data is always modified with respect to the corresponding tool parameters

($TC_DP2[..., ...] etc.) when the "Modification of the offset data for rotatable tools" function

was activated with the CUTMOD or CUTMODK command and the tool was rotated by an orientable

tool carrier or a suitable orientation transformation.

Further function-relevant system variables

System variable

Meaning

$P_CUTMOD_ANG /

Returns the angle through which a tool was rotated in the active machining

plane and the modified cutting edge data available for the CUTMOD and

$AC_CUTMOD_ANG

CUTMODK functions.

$P_CUTMOD /

Reads the currently valid value that was last programmed with the CUTMOD

command (number of the tool carrier for which the modification of the offset

$AC_CUTMOD

data should be activated).

If the last programmed value was CUTMOD = -2 (activation with the currently

active orientable tool carrier), then the value "-2" is not returned in the system

variable, but rather the number of the orientable tool carrier active at the time

of programming.

$P_CUTMODK /

Reads the name of the transformation under which the currently valid data set

for the "Modification of the offset data" was created.

$AC_CUTMODK

$P_CUT_INV /

Supplies the value TRUE if the tool is rotated so that the spindle direction of

rotation must be inverted. To do this, the following four conditions must be

$AC_CUT_INV

fulfilled in the block to which the read operations refer:

1. If a turning or grinding tool is active

(tool types 400 to 599 and / or SD42950 $SC_TOOL_LENGTH_TYPE = 2).

2. The modification of the offset data was activated with the CUTMOD or

CUTMODK command.

3. An orientable tool carrier or an orientation transformation defined with

kinematic chains is active, which was selected with the CUTMOD or

CUTMODK command.

4. The tool is rotated by the orientable tool carrier or the kinematic orientation

transformation so that the resulting normal of the tool cutting edge is

rotated with respect to the initial position by more than 90° (typically 180°).

If at least one of the specified four conditions is not fulfilled, the variable returns

the value FALSE. For tools whose cutting edge position is not defined, the

value of the variable is always FALSE.

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

463

Tool offsets

11.11 Modification of the offset data for rotatable tools

System variable

Meaning

$P_CUTMOD_ERR

Error state after the last call of the CUTMOD function

The CUTMOD function can also be called implicitly for a tool change. At a

reset, the variable is reset to zero. It is reset at every tool change and, if

required, rewritten.

The variable is bit-coded. The bits have the following meanings:

Bit 0:

No valid cut direction is defined for the active tool.

Bit 1:

The cutting edge angle (clearance angle and holder angle) of the

active tool are both zero.

Bit 2:

The clearance angle of the active tool has an impermissible value (<

0° or > 180°).

Bit 3:

The holder angle of the active tool has an impermissible value (< 0°

or > 90°).

Bit 4:

The plate angle of the active tool has an impermissible value (< 0° or

> 90°).

Bit 5:

The cutting edge position - holder angle combination of the active tool

is not permitted (the holder angle must be ≤ 90° for cutting edge po-

sition 1 to 4; for cutting edge positions 5 to 8 it must be ≥ 90°).

Bit 6:

Illegal rotation of the active tool.

The tool was rotated out of the active machining plane by ± 90° (with

a tolerance of about 1°). The cutting edge position is therefore no

longer defined in the machining plane.

Bit 7:

The cutting plate is not in the machining plane and the angle between

the cutting plate and the machining plane exceeds the upper limit

specified with the setting data SD42998 $SC_CUT-

MOD_PLANE_TOL.

Bit 8:

The cutting plate is not in the machining plane. Angle α is greater than

1°. Angle α is the angle of rotation around the coordinate axis which

is perpendicular to the axis of rotation of angle β as well as to the axis

of rotation of angle γ (the X axis for G18).

$P_...: Preprocessing variables

$AC_...: Main run variables

All main run variables can be read in synchronized actions. A read access operation from the

preprocessing generates a preprocessing stop.

Plane change

To determine the modified cutting edge position, cutting direction and holder or clearance

angle, the evaluation of the cutting edge in the active plane (G17 - G19) is decisive.

However, if setting data SD42940 $SC_TOOL_LENGTH_CONST (change of the tool length

component when selecting the plane) has a valid non-zero value (plus or minus 17, 18 or 19),

its contents define the plane in which the relevant quantities are evaluated.

This priority rule of the setting data over the G code can be deactivated by setting bit 18 of the

machine data $MC_TOOL_PARAMETER_DEF_MASK. This means that when this bit is set,

the plane defined with the G command of group 6 is still valid.

Job Planning

464

Programming Manual, 12/2018, A5E40869460B AB

Tool offsets

11.11 Modification of the offset data for rotatable tools

Effectiveness of the modified cutting data

The modified cutting edge position and the modified cutting edge reference point are

immediately effective when programming, even for a tool that is already active. A tool does

not have to be re-selected for this purpose.

;

%

r

=

r

6

r

3

6/

S:

Cutting edge center point

P:

Cutting edge reference point

SL:

Cutting edge position

Figure 11-4

Tool with cutting edge position 3 and an orientable tool carrier that can rotate the tool

around the B axis.

Program code

Comment

N10 $TC_DP1[1,1]=500

N20 $TC_DP2[1,1]=3

;Cutting edge position

N30 $TC_DP3[1,1]=12

N40 $TC_DP4[1,1]=1

N50 $TC_DP6[1,1]=6

N60 $TC_DP10[1,1]=110

; Holder angle

N70 $TC_DP11[1,1]=3

; Cut direction

N80 $TC_DP24[1,1]=25

; Clearance angle

N90 $TC_CARR7[2]=0 $TC_CARR8[2]=1 $TC_CARR9[2]=0

; B axis

N100 $TC_CARR10[2]=0 $TC_CARR11[2]=0

; C axis

$TC_CARR12[2]=1

N110 $TC_CARR13[2]=0

N120 $TC_CARR14[2]=0

N130 $TC_CARR21[2]=X

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

465

Tool offsets

11.12 Working with tool environments

<Status>:

Function return value. Negative values indicate error states.

Data type:

INT

Value:

0

Function OK

-1

No memory reserved for tool environments:

MD18116 $MN_MM_NUM_TOOL_ENV = 0

This means that the "tool environments" functionality is not

available.

-2

No more free memory locations for tool environments available.

-3

Null string illegal as name of a tool environment.

-4

No parameter (<name>) specified.

Parameters

1

<name>:

Name, under which the current data set should be saved.

If a data set of the same name already exists, then it is overwritten. In this case,

the status is "0".

Data type:

STRING

Additional information

Base dimension/adapter dimension - tool length compensation

When the tool magazine management is active (only available with the "Tool management"

option!), the value of the following machine data defines whether the adapter length or the tool

base dimension (cutting edge-specific parameters $TC_DP21, $TC_DP22 and $TC_DP23) is

incorporated in the calculation of the tool length:

MD18104 $MN_MM_NUM_TOOL_ADAPTER (tool adapter in TO area).

Since a change to this machine data only takes effect after the control system has powered

up, it is not saved in the tool environment.

Resulting length of toolholders with orientation capability and transformations:

Note

Both toolholders with orientation capability and transformations can use system variables or

machine data, which act as additional tool length components, and which can be subjected

partially or completely to the rotations performed. The resulting additional tool length

components must also be saved when TOOLENV is called, because they represent part of

the environment, in which the tool is used.

Adapter transformation

The adapter transformation is a property of the tool adapter and thus of the complete tool. It

is, therefore, not part of a tool environment, which can be applied to another tool.

By saving the complete data necessary to determine the overall tool length, it is possible to

calculate the effective length of the tool at a later point in time, even if the tool is no longer

active or if the conditions of the environment (e.g. G codes or setting data) have changed.

Similarly, the effective length of a different tool can be calculated assuming that it would be

used under the same conditions as the tool, for which the status was saved.

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

469

Tool offsets

11.12 Working with tool environments

Maximum number of data sets for tool environments

Machine data MD18116 $MN_MM_NUM_TOOL_ENV is used to define the maximum number

of data sets that can be saved to describe the tool environments. The data are in the TOA

area. They are kept even when the control system is switched off.

Data cannot be backed up. This means that this data cannot be transferred between the

different control systems.

11.12.2

Delete tool environment (DELTOOLENV)

The DELTOOLENV function is used to delete the data sets that are used to describe tool

environments. Deletion means that the set of data stored under a particular name can no longer

be accessed (an access attempt triggers an alarm).

Note

Data sets can only be deleted using the DELTOOLENV function, by an INITIAL.INI download

or by a cold start (NC power up with default machine data). There are no additional automatic

deletion operations.

Syntax

<Status> = DELTOOLENV(<name>)

<Status> = DELTOOLENV()

Meaning

DELTOOLENV(...):

Predefined function to delete a tool environment

Alone in the

Yes

block:

<Status>:

Function return value. Negative values indicate error states.

Data type:

INT

Value:

0

Function OK

-1

No memory reserved for tool environments:

MD18116 $MN_MM_NUM_TOOL_ENV = 0

This means that the "tool environments" functionality is not

available.

-2

A tool environment with the specified name does not exist.

Parameters

1

<name>:

Name of data set to be deleted

Data type:

STRING

DELTOOLENV():

DELTOOLENV() deletes data sets describing tool environments without spec-

ifying a name

Job Planning

470

Programming Manual, 12/2018, A5E40869460B AB

Tool offsets

11.12 Working with tool environments

11.12.3

Read T, D and DL number (GETTENV)

The GETTENV function is used to read the T, D and DL numbers stored in a tool environment.

Syntax

<Status> = GETTENV(<name>, <TDDL>)

Meaning

GETTENV(...):

Predefined function to read T, D and DL numbers in a data set to describe a tool

environment

Alone in the

Yes

block:

<Status>:

Function return value. Negative values indicate error states.

Data type:

INT

Value:

0

Function OK

-1

No memory reserved for tool environments:

MD18116 $MN_MM_NUM_TOOL_ENV = 0

This means that the "tool environments" functionality is not

available.

-2

A tool environment with the specified name does not exist.

Parameters

1

<name>:

Name of the data set from which the T, D and DL numbers are to be read

Data type:

STRING

2

<TDDL>:

The field of this result parameter contains the T, D and DL numbers of the tool,

whose tool environment is saved in the specified data set:

● <TDDL> [0]: T number

● <TDDL> [1]: D number

● <TDDL> [2]: DL number

Data type:

INT[3]

GETTENV(,<TDDL>),

When calling function GETTENV, it is permissible to omit the first pa-

GETTENV("",<TDDL>):

rameter - or to transfer the null string as first parameter. In these two

special cases, in <TDDL>, the T, D and DL numbers of theactive tool

are returned.

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

471

Tool offsets

11.12 Working with tool environments

11.12.4

Read information about the saved tool environments ($P_TOOLENVN,

($P_TOOLENV)

Information regarding the saved tool environments can be read using the following system

variables:

$P_TOOLENVN:

Supplies the number of data sets (which have still not been deleted) - defined

using TOOLENV - to describe tool environments

Syntax:

<n> = $P_TOOLENVN

Meaning:

<n>:

Number of defined data sets

Data type:

INT

Value range:

0 ... MD18116

$MN_MM_NUM_TOOL_ENV

This system variable can be accessed even if no tool environments are possible

(MD18116 = 0). In this case, the return value is "0".

$P_TOOLENV:

Supplies the name of the <i>th data set to describe a tool environment

Syntax:

<Name> = $P_TOOLENV[<i>]

Meaning:

<name>:

Name of the data set with number <i>

Data type:

STRING

<i>:

Number of the data set

Data type:

INT

Value range:

1 ... $P_TOOLENVN

The assignment of numbers to data sets is not fixed, but can be changed as a

result of deleting or creating data sets. The data sets are numbered internally.

If <i> refers to a data set that has not been defined, then the null string is returned.

If index <i> is not valid, i.e. <i> is less than 1 or higher than that the maximum

number of data sets for tool environments (MD18116 $MN_MM_NUM_TOO-

LENV), then the following alarm is output:

Alarm 17020 "inadmissible array index 1"

11.12.5

Read tool lengths and/or tool length components (GETTCOR)

The GETTCOR function is used to read out tool lengths or tool length components.

The parameters can be used to specify which components are considered and the conditions

under which the tool is used.

Syntax

<Status> = GETTCOR(<Len>[, <Comp>, <Stat>, <T>, <D>, <DL>])

Meaning

GETTCOR(...):

Predefined function to read tool lengths or to read tool length components

Alone in the

Yes

block:

Job Planning

472

Programming Manual, 12/2018, A5E40869460B AB

Tool offsets

11.12 Working with tool environments

<Status>:

Function return value. Negative values indicate error states.

Data type:

INT

Value:

0

Function OK

-1

No memory reserved for tool environments:

MD18116 $MN_MM_NUM_TOOL_ENV = 0

This means that the "tool environments" functionality is not

available.

-2

A tool environment with the name specified under <Stat> does

not exist.

-3

Invalid string in parameter <Comp>.

Causes of this error can be invalid characters or characters pro-

grammed twice.

-4

Invalid T number

-5

Invalid D number

-6

Invalid DL number

-7

Attempt to access a non-existent memory module.

-8

Attempt to access a non-existent option (programmable tool

orientation, tool management).

-9

The <Comp> string contains a colon (identifier for the specifi-

cation of a coordinate system), but it is not followed by a valid

character denoting the coordinate system.

Parameters

1

<Len>:

Result vector

Data type:

REAL[11]

The vector components are arranged in the following order:

● <Len> [0]: Tool type

● <Len> [1]: Cutting edge position

● <Len> [2]: Abscissa

● <Len> [3]: Ordinate

● <Len> [4]: Applicate

● <Len> [5]: Tool radius

The coordinate system defined in <Comp> and <Stat> is used as the reference

coordinate system for the length components. If a coordinate system is not defined

in <Comp>, then tool lengths are displayed in the machine coordinate system.

The assignment of the abscissa, ordinate and applicate to the geometry axes

depends on the active plane used in the tool environment. This means, for G17,

the abscissa is parallel to X, with G18 it is parallel to Z, etc.

Components <Len>[6] to <Len>[10] contain the additional parameters, which can

be used to specify the geometry description of a tool (e.g. $TC_DP7 to $TC_DP11

for the geometry and the corresponding components for wear or sum and setup

offsets).

These 5 additional elements and the tool radius are only defined for components

E, G, S, and W. Their evaluation does not depend on <Stat>. The corresponding

values in <Len>[6] to <Len>[10] can thus only be not equal to zero if at least one

of the four specified components is involved in the tool length calculation. The

remaining components do not influence the result. The dimensions refer to the

control's basic system (inch or metric).

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

473

Tool offsets

11.12 Working with tool environments

2

<Comp>:

Tool length components (optional)

Data type:

STRING

The character string consists of two substrings, which are separated from one

another by a colon.

General form: "<SubStr_1> [: <SubStr_2]"

<SubStr_1>:

The first substring designates the tool length components to be

taken into account when calculating the tool length.

The order of the characters in the substrings, and their notation

(upper or lower case), is arbitrary. Any number of blanks or

white spaces can be inserted between the characters.

Note:

It is not permissible that the characters in the substring are pro-

grammed twice.

Charac-

-

Minus symbol (only allowed as first character)

ters:

The complete tool length is calculated, minus

the components specified in the next string.

C

Adapter or tool base dimension (whichever of

the two alternative components is active for the

tool in use)

E

Setup offsets

G

Geometry

K

Kinematic transformation (is only evaluated for

generic 3, 4 and 5-axis transformation)

S

Summed offsets

T

Toolholder with orientation capability

W

Wear

If the first substring is empty (except for white spaces), the com-

plete tool length is calculated allowing for all components. This

applies even if the <Comp> parameter is not specified.

<Substr_2>:

The optional second substring identifies the coordinate system,

in which the tool length is to be output.

The second substring only comprises one single relevant char-

acter.

Charac-

A

Adjustable coordinate system (ACS)

ters:

B

Basic coordinate system (BCS)

K

Tool coordinate system of kinematic transfor-

mation (KCS)

M

Machine coordinate system (MCS)

T

Tool coordinate system (TCS)

W

Workpiece coordinate system (WCS)

If no coordinate system is specified, the evaluation is performed

in the MCS (machine coordinate system). If any rotations are

to be taken into account, they are specified in the tool environ-

ment defined in <Stat>.

3

<_Stat>:

Name of the data set for describing a tool environment (optional)

Data type:

STRING

If the value of this parameter is the null string (""), or is not specified, then the

current status is used. The current tool is used if a tool is not specified.

Job Planning

474

Programming Manual, 12/2018, A5E40869460B AB

Tool offsets

11.12 Working with tool environments

4

<T>:

Internal T number of the tool (optional).

Data type:

INT

If this parameter is not specified or if its value is "0", then the tool stored in <Stat>

is used.

If the value of this parameter is "-1", then the T number of the active tool is used.

It is also possible to explicitly specify the number of the active tool.

Note:

If <Stat> is not specified, the actual status is used as the tool environment. Since

<T> = 0 refers to the T number saved in the tool environment, the active tool is

used in this environment, i.e. parameters <T> = 0 and <T> = -1 have the same

meaning in this special case.

5

<D>:

Cutting edge of the tool (optional).

Data type:

INT

If this parameter is not specified, or if its value is "0", then the D number used is

based on the source of the T number. If the T number from the tool environment

is used, then the D number of the tool environment is also read, otherwise the D

number of the currently active tool is read.

6

<DL>:

Number of the offset dependent on the location (optional).

Data type:

INT

If this parameter is not specified, then the DL number used is based on the source

of the T number. If the T number from the tool environment is used, then the D

number of the tool environment is also read, otherwise the D number of the cur-

rently active tool is read.

Examples

GETTCOR(_LEN)

Calculates the tool length of the currently active

tool in the machine coordinate system allowing for

all components.

GETTCOR(_LEN,"CGW:W")

Calculates the tool length for the active tool, con-

sisting of the adapter or tool base dimension, ge-

ometry and wear. Further components, such as

toolholder with orientation capability or kinematic

transformation, are not considered. Output in the

workpiece coordinate system.

GETTCOR (_LEN,"-K:B")

Calculates the complete tool length of the active

tool without allowing for the length components of

a possibly active kinematic transformation. Output

in the basic coordinate system.

GETTCOR (_LEN,":M","Testenv1",,3)

Calculates the complete tool length in the machine

coordinate system for the tool stored in the tool

environment named "Testenv1". However, the cal-

culation is performed for cutting edge number D3,

regardless of the cutting edge number stored.

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

475

Tool offsets

11.12 Working with tool environments

Additional information

Adapter transformation/toolholder with orientation capability/kinematic transformation

Any rotations and component exchanges initiated by the adapter transformation, toolholder

with orientation capability and kinematic transformation, are part of the tool environment. They

are thus always performed, even if the corresponding length component is not supposed to

be included. If this is undesirable, tool environments must be defined, in which the

corresponding transformations are not active. In many cases (i.e. any time a transformation

or toolholder with orientation capability is not used on a machine), the data sets stored for the

tool environments automatically fulfill these conditions, with the result that the user does not

need to make special provision.

Turning and grinding tools: Calculating the tool length depending on MD20360

$MC_TOOL_PARAMETER_DEF_MASK

The following machine data defines how the wear and tool length are to be evaluated if a

diameter axis is used for turning and grinding tools.

MD20360 $MC_TOOL_PARAMETER_DEF_MASK (definition of tool parameters).

Bit

Value

0

For turning and grinding tools, the wear parameter of the transverse axis is taken into account

as the diameter value:

= 0 (default)

No

= 1

Yes

1

For turning and grinding tools, the tool length component of the transverse axis is taken into

account as the diameter value:

= 0 (default)

No

= 1

Yes

If the bits involved are set, the associated entry is weighted with a factor of 0.5. This weighting

is reflected in the tool length returned by GETTCOR.

Example:

MD20360 $MC_TOOL_PARAMETER_DEF_MASK = 3

MD20100 $MC_DIAMETER_AX_DEF (geometry axis with transverse axis function) = "X"

X is diameter axis (standard turning machine configuration)

Program code

Comment

N30 $TC_DP1[1,1]=500

N40 $TC_DP2[1,1]=2

N50 $TC_DP3[1,1]=3.0

; geometry L1

N60 $TC_DP4[1,1]=4.0

N70 $TC_DP5[1,1]=5.0

N80 $TC_DP12[1,1]=12.0

; wear L1

N90 $TC_DP13[1,1]=13.0

N100 $TC_DP14[1,1]=14.0

N110 T1 D1 G18

N120 R1=GETTCOR(_LEN,"GW")

N130 R3=_LEN[2]

; 17.0 (= 4.0 + 13.0)

Job Planning

476

Programming Manual, 12/2018, A5E40869460B AB

Tool offsets

11.12 Working with tool environments

Program code

Comment

N140 R4=_LEN[3]

; 7.5 (= 0.5 * 3.0 + 0.5 * 12.0)

N150 R5=_LEN[4]

; 19.0 (= 5.0 + 14.0)

N160 M30

Length components of the kinematic transformation and toolholder with orientation capability

If a toolholder with orientation capability is taken account of during the tool length calculation,

the following vectors are included in that calculation:

Type

Vectors

M

l1 and l2

T

l1, l2 and l3

P

The tool length is not influenced by the toolholder with orientation capability.

In generic 5-axis transformation, the following machine data are included in the tool length

calculation for transformer types 24 and 56:

Transforma-

Machine data

tion type

24

MD24550/24650 $MC_TRAFO5_BASE_TOOL_1/2

MD24560/24660 $MC_TRAFO5_JOINT_OFFSET_1/2

MD24558/24658 $MC_TRAFO5_PART_OFFSET_1/2

56

MD24550/24650 $MC_TRAFO5_BASE_TOOL_1/2

MD24560/24660 $MC_TRAFO5_JOINT_OFFSET_1/2

Transformation type 56 (moving tool and moving workpiece) corresponds to type M for

toolholders with orientation capability.

For this 5-axis transformation, in the previous software releases, vector MD24560/24660

$MC_TRAFO5_JOINT_OFFSET_1/2 (vector of kinematic offset of the 1st/2nd 5-axis

transformation in the channel) corresponds to the sum of the two vectors l₁ and l₃ for a type

M tool carrier with orientation capability.

Only the sum is relevant for the transformation in both cases. The way, in which the two

individual components are composed, is insignificant. However, when calculating the tool

length, it is relevant which component is assigned to the tool and which is assigned to the tool

table. This is the reason that machine data MD24558/24658

$MC_TRAFO5_JOINT_OFFSET_PART_1/2 (vector kinematic offset in table) was introduced.

It corresponds to vector l3. Machine data:MD24560/24660

$MC_TRAFO5_JOINT_OFFSET_1/2 no longer corresponds to the sum of l1 and l3, but only

to vector l1. If machine data MD24558/24658 $MC_TRAFO5_JOINT_OFFSET_PART_1/2 is

equal to zero, the behavior is the same as before.

Compatibility

The GETTCOR function is used in conjunction with the TOOLENV and SETTCOR functions

to replace parts of the functionality, which were previously implemented externally in the

measuring cycles.

Only some of the parameters, which actually determine the effective tool length, were

implemented in the measuring cycles. The functions mentioned above can be configured to

reproduce the behavior of the measuring cycles in relation to the tool length calculation.

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

477

Tool offsets

11.12 Working with tool environments

<Status>:

Function return value. Negative values indicate error states.

Data type:

INT

Value:

0

Function OK

-1

No memory reserved for tool environments:

MD18116 $MN_MM_NUM_TOOL_ENV = 0

This means that the "tool environments" functionality is not

available.

-2

A tool environment with the name specified under <Stat> does

not exist.

-3

Invalid string in parameter <Comp>.

Causes of this error can be invalid characters or characters pro-

grammed twice.

-4

Invalid T number.

-5

Invalid D number.

-6

Invalid DL number.

-7

Attempt to access a non-existent memory module.

-8

Attempt to access a non-existent option (programmable tool

orientation, tool management).

-9

Illegal numerical value for parameter <CorComp>.

-10

Illegal numerical value for parameter <CorMode>.

-11

The contents of parameters <Comp> and <CorComp> are con-

tradictory.

-12

The contents of parameters <Comp> and <CorMode> are con-

tradictory.

-13

The content of the <GeoAx parameter does not designate a

geometry axis.

-14

Write attempt to a non-existent setup offset.

Parameters

1

<CorVal>:

Correction vector

In the workpiece coordinate system (WCS) defined by <Stat>, the following as-

signment applies:

● <CorVal> [0]: Abscissa

● <CorVal> [1]: Ordinate

● <CorVal> [2]: Applicate

If only one tool component is to be corrected (i.e. no vectorial correction, see

parameter <CorMode>), the correction value is always in <CorVal>[0], independ-

ent of the axis on which it acts. The contents of the other two components are then

not evaluated.

If <CorVal> or a component of <CorVal> refers to the transverse axis, then the

data is evaluated as radius dimension. This means that a tool is, for example,

"longer" by the specified dimension; this correspondingly results in a change to

the workpiece diameter that is twice as large.

The dimensions refer to the basic system (inch or metric) of the control system.

Data type:

REAL[3]

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

479

Tool offsets

11.12 Working with tool environments

2

<Comp>:

Tool component(s)

Data type:

STRING

The character string consists of two substrings, which are separated from one

another by a colon.

General form: "<SubStr_1> [: <SubStr_2]"

<SubStr_1>:

The first substring must always be available, and can either

comprise one or two characters. The first or only character for

the 1st component (Val₁) and the second character for the 2nd

component (Val₂), which are processed according to the sub-

sequent parameters <CorComp> and <CorMode>.

Charac-

C

Adapter or tool base dimension (whichever

ters:

of the two alternative components is active

for the tool in use)

E

Setup offsets

G

Geometry

S

Sum offsets

W

Wear

<Substr_2>:

The second substring is optional. Alternatively, it can comprise

(individual) letters "W" or "T".

Charac-

W

If the second substring is empty or contains

ters:

the letter "W", then the offset values are

taken into account as if they had been

measured in the workpiececoordinate sys-

tem (WCS).

T

If the second substring contains the letter

"T", then the offset values are taken into

account as if they had been measured in

the toolcoordinate system (Tool Coordinate

System, TCS).

The notation of the characters in the string (upper or lower case) is arbitrary. Any

number of spaces or tabs (white spaces) can be inserted.

Job Planning

480

Programming Manual, 12/2018, A5E40869460B AB

Tool offsets

11.12 Working with tool environments

3

<CorComp>:

Specifies the component(s) of the tool data sets that are to be described (optional).

Data type:

INT

Value:

0

Offset value <CorVal>[0] refers to the geometry axis transferred

in parameter <GeoAx> in the workpiece coordinate system - or

in the tool coordinate system (also see a description of param-

eter <Comp>). This means that the offset value must be calcu-

lated in the designated tool components so that, taking account

all the parameters that can influence the tool length calculation,

a change of the total tool length by the specified value in the

specified axis direction is obtained.

This change should be achieved by correcting the component

specified in <Comp> and the symbolic algorithm specified in

<CorMode> (see the following parameters). The resulting cor-

rection can therefore have an effect on all three axis compo-

nents.

1

Like "0", however, vectorial. The content of vector <CorVal>

refers to abscissa, ordinate and applicate in the workpiece co-

ordinate system or tool coordinate system (see the description

of parameter <Comp>).

Subsequent parameter <GeoAx> is not evaluated.

2

Vectorial offset, i.e. L1, L2 and L3 can change simultaneously.

In contrast to the versions from "0 and "1", the offset values

contained in <CorVal> refer to the coordinates of Val₁ compo-

nents (see following parameter <CorMode>) of the tool.

Any possible inclination of an existing tool compared with the

workpiece coordinate system has no influence on the offset.

3 - 5

Correction of tool lengths L1 to L3 ($TC_DP3 to $TC_DP5) or

the corresponding values for wear, setting up or additive offsets.

The offset value is contained in <CorVal>[0]. It is measured in

the coordinates of the Val₁ component (see following parameter

<CorMode>) of the tool. Any possible inclination of an existing

tool compared with the workpiece coordinate system has no

influence on the offset.

6

Correction of the tool radius ($TC_DP6) or the corresponding

values for wear, setting up or additive offsets. Bits 10 and 11

(evaluation of the diameter and/or diameter wear data, either

specified as a radius or diameter) in machine data

MD20360 $MC_TOOL_PARAMETER_DEF_MASK are taken

into account.

7 -

Correction of $TC_DP7 to $TC_DP11 or the corresponding val-

11

ues for wear, setting up or additive offsets. These parameters

are treated just like the tool radius.

If this parameter is not specified then its value is "0".

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

481

Tool offsets

11.12 Working with tool environments

4

<CorMode>:

Specifies the type of write operation to be executed (optional).

Data type:

INT

Value:

0

Val_1new = <CorVal>

1

Val_1new = Val_1old + <CorVal>

2

Val_1new = <CorVal>

Val_2new = 0

3

Val_1new = Val_1old + Val_2old + <CorVal>

Val_2new = 0

The notation Val_1old + Val_2old is symbolic. If the two components (due to the status

of <_Stat>) are evaluated in different ways, i.e. if a rotation is effective between

the two components, then Val_2old is transformed prior to addition so that the result-

ing tool length after deleting Val_2new and prior to the addition of <CorVal> remains

unchanged.

<CorVal> always refers to Val₁. <CorVal> is a value, which dependent on the

second part of parameter <Comp>, is measured in the workpiece coordinate sys-

tem (WCS) or in the tool coordinate system (TCS). It is therefore already trans-

formed with respect to the tool components, in which it should be calculated.

Therefore, it cannot be directly calculated together with the saved value, but must

be transformed back prior to adding to Val₁ or Val₂. This can mean that the offset

acts on an axis different than the one defined by <CorComp> - or that it acts on

several axes.

For the case <CorComp> = 0, i.e. when <CorVal> does not contain a vector, but

only an individual value, then the described operations are executed in the coor-

dinates in which <CorVal> was measured (WCS/TCS). In particular, this also ap-

plies to setting Val_2new to zero in variants 2 and 3. This result is then transformed

back into the coordinates of the tool. This can mean that none of the coordinate

values to be set to zero (L1, L2, L3) become zero, or coordinate values, that were

previously zero, are now not equal to zero. However, if the corresponding opera-

tions are successively executed for all three geometry axes, then it is guaranteed

that all three coordinate values of the components to be deleted are zero. If the

tool is not rotated with respect to the workpiece coordinate system or is rotated

so that all tool components remain parallel to the coordinate axes (axis exchange

operations), then this also ensures that only one tool coordinate changes.

The successive execution of the same operation (<CorMode>) with <Cor-

Comp> = 0 for all three coordinate axes in any sequence is identical with the single

execution of the same operation with <CorComp>=1.

For parameter values "0" and "1", parameter <Comp> must contain one character,

and for parameter values "2" and "3", two characters.

Example:

<Comp> contains string "ES", <CorMode> the value "2"

⇒ Setup offset_new = <CorVal>, summed offset_new = 0

If parameter <CorMode> is not specified, then its value is "0".

5

<GeoAx>:

Specifies the index of the geometry axis in which the offset value <CorVal>[0] was

read (optional)

Data type:

INT

Value range:

0 ... 2

Indices 0 to 2 refer to abscissa, ordinate and applicate in the active plane (G17/

G18/G19) of the current tool environment.

The content of this parameter is only evaluated if parameter <CorComp> has a

value of "0".

Job Planning

482

Programming Manual, 12/2018, A5E40869460B AB

Tool offsets

11.12 Working with tool environments

6

<Stat>:

Name of the data set for describing a tool environment (optional)

Data type:

STRING

If the value of this parameter is the null string (""), or is not specified, then the

current status is used. The current tool is used if a tool is not specified.

7

<T>:

Internal T number of the tool (optional).

Data type:

INT

If this parameter is not specified or if its value is "0", then the tool stored in <Stat>

is used.

If the value of this parameter is "-1", then the T number of the active tool is used.

It is also possible to explicitly specify the number of the active tool.

Note:

If <Stat> is not specified, the actual status is used as the tool environment. Since

<T> = 0 refers to the T number saved in the tool environment, the active tool is

used in this environment, i.e. parameters <T> = 0 and <T> = -1 have the same

meaning in this special case.

8

<D>:

Cutting edge of the tool (optional).

Data type:

INT

If this parameter is not specified, or if its value is "0", then the D number used is

based on the source of the T number. If the T number from the tool environment

is used, the D number of the tool environment is also read, otherwise the D number

of the currently active tool is read.

9

<TL>:

Number of the offset dependent on the location (optional).

Data type:

INT

If this parameter is not specified, then the DL number used is based on the source

of the T number. If the T number from the tool environment is used, the D number

of the tool environment is also read, otherwise the D number of the currently active

tool is read. If T, D and DL specify a tool without location-dependent offsets, no

summed or setup offsets may be specified in parameter <Comp> (error code in

<Status>).

Note

Not all possible combinations of the three parameters <Comp>, <CorComp> and <CorMode>

make sense. For example, algorithm 3 in <CorComp> requires that two characters are

specified in <Comp>. If an invalid parameter combination is specified, then a corresponding

error code is returned in the <Status>.

Examples

Example 1

Program code

Comment

N10 DEF REAL _CORVAL[3]

N20 $TC_DP1[1,1]=120

; Milling tool

N30 $TC_DP3[1,1]=10.0

; Geometry L1

N40 $TC_DP12[1,1]=1.0

; wear L1

N50 _CORVAL[0]=0.333

N60 T1 D1 G17 G0

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

483

Tool offsets

11.12 Working with tool environments

G18 is active. Since <CorMode> = 3, the tool wear in the direction of the X axis of the WCS

must become zero once N100 has been executed.

The contents of the relevant tool parameters at the end of the program are thus:

$TC_DP3[1,1]: 21.830 ; geometry L1

$TC_DP4[1,1] : 21.830 ; geometry L2

$TC_DP12[1,1] : 2.500 ; wear L1

$TC_DP13[1,1] : -4.330 ; wear L2

The geometrical relationships are shown in the figure below: The total wear including

_CORVAL is mapped onto the X' direction in the WCS. This produces point P2. The

coordinates of this point (measured in X/Y coordinates) are entered in the geometry component

of the tool. The difference vector P₂ - P₁ remains in the wear. The wear thus no longer has a

component in the direction of _CORVAL.

2ULJLQDO WRRO OHQJWK

[

[

3

B&259$/ DFWLYH LQ WKH ; GLUHFWLRQ

:HDU /

/

*HRPHWU\ /

/

]

If the program example is continued after N110 with the following instructions, then the

remaining wear is included completely in the geometry because the compensation is now

effective in the Z' axis (parameter <GeoAx> = 0):

N120 _CORVAL[0]=0.0

N130 R1=SETTCOR(_CORVAL,"GW",0,3,0)

N140 T1 D1 X0 Y0 Z0 ; ==> MCS position X24.330 Y0.000 Z17.500

Since the new compensation value is "0", the total tool length and thus the position approached

in N140 may not change. If _CORVAL were not equal to "0" in N120, a new total tool length

and thus a new position in N140 would result, however, the wear component of the tool length

would always be zero, i.e. the total tool length is subsequently always contained in the

geometry component of the tool.

Job Planning

486

Programming Manual, 12/2018, A5E40869460B AB

Tool offsets

11.12 Working with tool environments

Example 8

Program code

Comment

N10 DEF REAL _CORVAL[3]

N20 $TC_DP1[1,1]=500

; turning tool

N30 $TC_DP3[1,1]=10.0

; geometry L1

N40 $TC_DP4[1,1]=15.0

; geometry L2

N50 $TC_DP5[1,1]=20.0

; geometry L3

N60 $TC_DP12[1,1]=10.0

; wear L1

N70 $TC_DP13[1,1]=0.0

; wear L2

N80 $TC_DP14[1,1]=0.0

; wear L3

N90 $SC_WEAR_SIGN=TRUE

N100 _CORVAL[0]=10.0

N110 _CORVAL[1]=15.0

N120 _CORVAL[2]=5.0

N130 ROT Y-30

N140 T1 D1 G18 G0

N150 R1=SETTCOR(_CORVAL,"W",1,1)

N160 T1 D1 X0 Y0 Z0

; ==> MCS position X7.990 Y25.000 Z31.160

N170 M30

Setting data:SD42930 $SC_WEAR_SIGN is enabled in N90, i.e. the wear must be evaluated

with a negative sign. The compensation is vectorial (<CorComp> = 1), and the compensation

vector must be added to the wear (<CorMode> = 1). The geometrical relationships in the Z/X

plane are shown in the diagram below:

;

;

5HVXOWLQJ ZHDU FRPSRQHQW

*HRPHWU\

/

/

3

3

B&259$/ <

;

=

3

=

:HDU /

/

2ULJLQDO WRRO OHQJWK

QHJDWLYH HYDOXDWLRQ

=

The geometry component of the tool remains unchanged due to <CorMode> = 1. The

compensation vector defined in the WCS (rotation around the y axis) must be included in the

wear component such that the total tool length in Fig. 3 refers to point P₂. Therefore, the

resulting wear component of the tool is given by the distance of the two points P₁ and P₂.

Job Planning

488

Programming Manual, 12/2018, A5E40869460B AB

Content      ..     5      6      7      8     ..