Content      ..     4      5      6      7     ..

SINUMERIK 840D sl/828D. Job Planning. Programming Manual (2010-2018) - page 6

Transformations

7.5 Orientations relative to the path

N... TILT=

Angle for the programmed orientation in the plane,

vertical to the path tangent relative to the surface

normal vector

N... THETA=

Angle of rotation relative to the change of orientation

in the tool direction of the third rotary axis

The values of the angles at the end of block are programmed using LEAD=value,

TILT=value or THETA=value. In addition to the constant angles, polynomials can be

programmed for all three angles up to the 5th degree.

N... PO[PHI]=(a2, a3, a4, a5)

Polynomial for the leading angle LEAD

Polynomial for the tilt angle TILT

N... PO[PSI]=(b2, b3, b4, b5)

Polynomial for the angle of rotation THE-

N... PO[THT]=(d2, d3, d4, d5)

TA

The higher polynomial coefficients, which are zero, can be omitted when programming.

Example: PO[PHI]=a2 results in a parabola for the LEAD angle.

Meaning

Tool orientation relative to the path

ORIPATH:

Tool orientation in relation to path

ORIPATHS

Tool orientation in relation to path, blips in the orientation characteristic are smoothed

:

LEAD:

Angle relative to the surface normal vector in the plane that is defined by the path tangent

and the surface normal vector

TILT:

Rotation of orientation in the Z direction or rotation about the path tangent

THETA:

Rotation about the tool direction toward Z

PO[PHI]:

Orientation polynomial for the LEAD angle

PO[PSI]:

Orientation polynomial for the TILT angle

PO[THT]:

Orientation polynomial for the THETA angle of rotation

Note

Angle of rotation THETA

A 6-axis transformation is required to rotate a tool with a third rotary axis that acts as an

orientation axis about itself.

7.5.3

Interpolation of the tool rotation relative to the path (ORIROTC, THETA)

Interpolation with rotation vectors

The rotation vector of the tool rotation, programmed with ORIROTC, relative to the path tangent

can also be interpolated with an offset that can be programmed using the THETA angle of

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

351

Transformations

7.5 Orientations relative to the path

ORIAXES:

Linear interpolation of machine or orientation axes

ORIVECT:

Large-circle interpolation (identical to ORIPLANE)

ORIMKS:

Rotation in the machine coordinate system

ORIWKS:

Rotation in the workpiece coordinate system

Description, see the Rotations of the tool orientation section

A= B= C=:

Programming the machine axis position

ORIEULER:

Orientation programming via Euler angle

ORIRPY:

Orientation programming via RPY angle

A2= B2= C2=:

Angle programming of virtual axes

ORIVIRT1:

Orientation programming using virtual orientation axes

ORIVIRT2:

(definition 1), definition according to MD $MC_ORIAX_TURN_TAB_1

(definition 2), definition according to MD $MC_ORIAX_TURN_TAB_2

A3= B3= C3=:

Direction vector programming of direction axis

ORIPLANE:

Interpolation in the plane (large-circle interpolation)

ORICONCW:

Interpolation on the peripheral surface of a taper in the clockwise direc-

tion

ORICONCCW:

Interpolation on the peripheral surface of a taper in the counter-clock-

wise direction

ORICONTO:

Interpolation on the peripheral surface of a taper with tangential transition

A6= B6= C6=:

Programming of a rotary axis of the taper (normalized vector)

NUT=angle

Opening angle of taper in degrees

NUT=+179

Traverse angle less than or equal to 180 degrees

NUT=-181

Traverse angle greater than or equal to 180 degrees

ORICONIO:

Interpolation on the peripheral surface of a taper

A7= B7= C7=:

Intermediate orientation (programming as normalized vector)

ORICURVE

Interpolation of the orientation specifying a movement between two con-

tact points of the tool. In addition to the end points, additional curve

XH YH ZH, e.g. with

polynomials can also be programmed.

polynomials

PO[XH]=(xe, x2, x3,

x4, x5)

Note

If the tool orientation with active ORIAXES is interpolated via the orientation axes, the angle

of rotation is only initiated relative to the path at the end of block.

7.5.4

Smoothing of orientation characteristic (ORIPATHS A8=, B8=, C8=)

Changes of orientation that take place with constant acceleration on the contour can cause

unwanted interruptions to the path motions, particularly at the corner of a contour. The resulting

blip in the orientation characteristic can be smoothed by inserting a separate intermediate

block. If ORIPATHS is active during reorientation, the change in orientation occurs at a

constant acceleration. The tool can be retracted in this phase.

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

353

Transformations

7.5 Orientations relative to the path

Machine manufacturer

Please refer to the machine manufacturer's notes on any predefined machine and setting data

used to activate this function.

Machine data can be used to set how the retracting vector is interpreted:

1. In the TCS, the Z coordinate is defined by the tool direction.

2. In the WCS, the Z coordinate is defined by the active plane.

For further explanations about the "Orientation relative to the path" function , see

References:

Function Manual, Special Functions; Multi-axis Transformations (F2)

Syntax

Further programming details are needed at the corner of the contour for constant tool

orientations relative to the path as a whole. The direction and path length of this motion is

programmed via the vector using the components A8=X, B8=Y C8=Z.

N... ORIPATHS A8=X B8=Y C8=Z

Meaning

ORIPATHS:

Tool orientation relative to the path; blip in orientation characteristic is smoothed

A8= B8= C8=:

Vector components for direction and path length

X, Y, Z:

Retracting movement in tool direction

Note

Programming direction vectors A8, B8, C8

If the length of this vector is exactly zero, no retracting movement is executed.

ORIPATHS

Tool orientation relative to the path is activated using ORIPATHS. The orientation is otherwise

transferred from the start orientation to the end orientation by means of linear large-circle

interpolation.

Job Planning

354

Programming Manual, 12/2018, A5E40869460B AB

Transformations

7.8 Kinematic transformation

7.8

Kinematic transformation

7.8.1

Activate face end transformation (TRANSMIT)

The front face transformation (TRANSMIT) is activated in the part program or synchronized

action using the TRANSMIT statement.

Syntax

TRANSMIT

TRANSMIT(<n>)

Meaning

TRANSMIT:

Activate TRANSMIT with the first TRANSMIT data set

TRANSMIT(n):

Activate TRANSMIT with the nth TRANSMIT data set

Note

A TRANSMIT transformation active in the channel is activated with:

● Deactivate transformation: TRAFOOF

● Activation of another transformation: E.g. TRACYL, TRAANG, TRAORI

7.8.2

Activate cylinder surface transformation (TRACYL)

The cylinder surface transformation (TRACYL) is activated in the part program or synchronized

action using the TRACYL statement.

Syntax

TRACYL(<d>)

TRACYL(<d>,<n>)

TRACYL(<d>,<n>,<k>)

Meaning

TRACYL(<d>):

Activate TRACYL with the first TRACYL data set and working diameter

<d>

TRACYL (<d>,<n>):

Activate TRACYL with the <n>th TRACYL data set and working diameter

<d>

<d>:

Reference or working diameter

The value must be greater than 1.

Job Planning

360

Programming Manual, 12/2018, A5E40869460B AB

Transformations

7.8 Kinematic transformation

<n>:

TRACYL data set number (optional)

Range of values:

1, 2

<k>:

The parameter <k> is only relevant for transformation type 514

k = 0:

without groove side correction

k = 1:

with groove side correction

If the parameter is not specified, then the parameterized basic position

applies:

$MC_TRACYL_DEFAULT_MODE_<n>

With <n> = TRACYL data set number

Note

A TRACYL transformation active in the channel is switched-off with:

● Deactivate transformation: TRAFOOF

● Activation of another transformation: E.g. TRAANG, TRANSMIT, TRAORI

Example

Program code

Comment

N40 TRACYL(40.)

; Activate TRACYL with the first TRACYL data set

and working diameter 40 mm.

Further information

Program structure

A part program for milling a groove with TRACYL transformation 513 (TRACYL with groove

side offset) generally comprises the following steps:

1. Select tool.

2. Select TRACYL.

3. Select suitable coordinate offset (frame).

4. Positioning.

5. Program OFFN.

6. Select TRC.

7. Approach block (position TRC and approach groove side).

8. Groove center line contour.

9. Deselect TRC.

10.Retraction block (retract TRC and move away from groove side).

11.Positioning.

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

361

Transformations

7.8 Kinematic transformation

12.TRAFOOF.

13.Reselect original coordinate shift (frame).

Contour offset (OFFN)

In order to mill grooves using TRACYL transformation 513, the center line of the groove and

half of the groove width via the OFFN address are programmed in the part program.

To avoid damage to the groove side, OFFN acts only when the tool radius compensation is

active.

It is possible to change OFFN within a part program. This allows the groove center line to be

offset from the center:

2))1

3URJUDPPHG SDWK

Note

OFFN should be at least as large as the tool radius to avoid damage occurring to the opposite

side of the groove wall.

Note

OFFN acts differently with TRACYL than it does without TRACYL. Since, even without

TRACYL, OFFN is included when TRC is active, OFFN should be reset to zero after TRAFOOF.

NOTICE

Effect of OFFN depends on the transformation type

For TRACYL transformation 513 (TRACYL with groove side offset), half the groove width is

programmed for OFFN.

For TRACYL transformation 512 (TRACYL with groove side offset), the value of OFFN acts

as an allowance for the TRC.

Job Planning

362

Programming Manual, 12/2018, A5E40869460B AB

Transformations

7.8 Kinematic transformation

Tool radius compensation (TRC)

For TRACYL transformation 513, the TRC is not taken into account relative to the groove side,

but to the programmed center of the groove. In order that the tool travels to the left of the

groove side, statement G42 must be programmed instead of G41 or the value of OFFN

specified with a negative sign.

Tool diameter

With TRACYL and a tool whose diameter is less than the groove width, the same groove side

geometry is not generated as with a tool whose diameter is the same as the groove width. To

improve the precision, it is recommended that the tool diameter is selected to be only slightly

less than the groove width.

Axis utilization

Note

The following axes cannot be used as a positioning axis or a reciprocating axis:

● The geometry axis in the peripheral direction of the cylinder peripheral surface (Y axis).

● The additional linear axis for groove side compensation (Z axis).

7.8.3

Activating an oblique angle transformation with programmable angle (TRAANG)

The oblique angle transformation with programmable angle is activated in the part program or

synchronized action using the TRAANG statement.

Syntax

TRAANG

TRAANG()

TRAANG(, <n>)

TRAANG(<α>)

TRAANG(<α>,<n>)

Meaning

TRAANG:

Activate TRAANG with the first TRAANG data set and last valid angle

<α>

TRAANG():

TRAANG(, <n>):

Activate TRAANG with the <n>th TRAANG data set and last valid angle

<α>

TRAANG(<α>):

Activate TRAANG with the first TRAANG data set and angle <α>

TRAANG(<α>,<n>):

Activate TRAANG with the <n>th TRAANG data set and angle <α>

<α>:

Angle of the inclined axis (optional)

Range of values:

-90° < α < + 90°

The initial state parameterized in the machine data is effective if an

angle is not specified:

MD2xxxx $MC_TRAANG_ANGLE_<n>

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

363

Transformations

7.8 Kinematic transformation

<n>:

TRAANG data set number (optional)

Range of values:

1, 2

Note

Oblique angle transformation TRAANG active in the channel is deactivated using:

● Deactivate transformation: TRAFOOF

● Activation of another transformation: E.g. TRACYL, TRANSMIT, TRAORI

Example

Program code

Comment

N20 TRAANG(45)

; Activate TRAANG with the first TRAANG data set and angle 45°

7.8.4

Oblique plunge-cutting on grinding machines (G5, G7)

The G commands G7 and G5 are used to simplify programming of oblique plunge-cutting on

grinding machines with "inclined axis (TRAANG)", so that when plunge cutting, only the inclined

axis is traversed.

Only the required end position of the plunge-cutting motion has to be programmed in X and

Z. For G7, starting from the actual position of the X axis, the NC calculates and approaches

the programmed end position and angle α of the inclined axis.

The starting position is calculated from the point where the two straight lines intersect:

● Straight line parallel to the Z axis, at a distance from the actual position of the X axis

● Straight line parallel to the inclined axis through the programmed end position

With the subsequent G5, the inclined axis is traversed to the programmed end position.

Syntax

G7 <Endpos_X> <Endpos_Z>

G5 <Endpos_X>

Meaning

G7:

Calculate the starting position for the oblique plunge-cutting and approach.

G5:

Traverse the inclined axis to the programmed end position

<Endpos_X>:

X axis end position

<Endpos_Z>:

End position of the Z axis

Job Planning

364

Programming Manual, 12/2018, A5E40869460B AB

Transformations

7.8 Kinematic transformation

Example

˞

80

*ULQGLQJ ZKHHO

;

1

&0

1

$60

=

=0

:RUNSLHFH

① Parallel to the Z axis, at a distance from the actual position of the X axis

② Parallel to the inclined axis through the programmed end position

③ Starting position

④ Plunge-cutting: Starting position

⑤ Plunge-cutting: End position

X

Geometry axis

Z

Geometry axis

ZM Machine axis

UM Machine axis

Program code

Comment

N... G18

; Select XZ plane.

N40 TRAANG (45.0)

; Activate TRAANG transformation, angle = 45°

N50 G7 X40 Z70 F4000

; Calculate the starting position and approach

N60 G5 X40 F100

; Traverse inclined axis to the end position.

N70 ...

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

365

Transformations

7.9 Activate concatenated transformation (TRACON)

7.9

Activate concatenated transformation (TRACON)

A configured concatenated (chained) transformation is activated in the part program or

synchronized action using the TRACON statement.

Syntax

TRACON(<Trafo_No>,<Par_1>,...,<Par_n>,<Par_n+1>)

TRAFOOF

Meaning

TRACON:

Activate concatenated transformation

If another transformation was previously activated, it is implicitly dis-

abled by means of TRACON().

<Trafo_No>:

Number of the concatenated transformation:

Type:

INT

Range of val-

0 ... 2

ues:

Value:

0, 1

First/only concatenated transformation

2

Second concatenated transformation

Not

Same meaning as with 0 or 1

speci-

fied

Note:

Values not equal to 0, 1, 2 generate an error

alarm.

<Par_1>, ..., <Par_n>,

Parameters for the concatenated transformations

<Par_n+1>:

<Par_1>, ..., <Par_n>

Parameters of the first transforma-

tion in the chain

The actual number depends on

the transformation type:

● TRAORI: 2 parameters

● TRACYL: 1 to 2 parameters

<Par_n+1>

Parameters of the second transfor-

mation in the chain (TRAANG)

≙ angle of the inclined axis

If parameters are not set, the defaults or the parameters last used

take effect. Commas must be used to ensure that the specified pa-

rameters are evaluated in the sequence in which they are expected,

if default settings are to be effective for previous parameters. In

particular, a comma is required before at least one parameter, even

though it is not necessary to specify <Trafo_No> - for example TRA-

CON( , 3.7).

TRAFOOF:

Deactivate the last activated (concatenated) transformation

Job Planning

366

Programming Manual, 12/2018, A5E40869460B AB

Transformations

7.10 Cartesian PTP travel

$

$

$

$

$

$

Axes A1, A2 and A3 are the main axes of the articulated robot. The axes A4, A5 and A6, which

are also designated as head or hand/wrist axes, are positioned in the working area with the

main axes. The additional motion options of the hand/wrist axes enable the milling spindle to

be orientated in space as required for the particular machining task. Various articulated joint

positions are possible to achieve the same tool orientation.

The articulated joint positions required for machining are selected by programming bit 0 ... 2

of the adjustable STAT address:

Bit 0

Position of the intersection points of the hand/wrist axes (A4, A5, A6)

= 0

Basic range (shoulder right)

The robot is in the basic range if the X value

of the intersection point of the hand/wrist ax-

es is positive in relation to to the A1 coordi-

nate system.

= 1

Overhead range (shoulder left)

%LW

%LW

The robot is in the overhead range if the X

value of the intersection point of the hand/

wrist axes is negative in relation to the A1

coordinate system.

;

;

$

Example: The intersection point of

the hand/wrist axes lies in the basic

range

Job Planning

370

Programming Manual, 12/2018, A5E40869460B AB

Transformations

7.10 Cartesian PTP travel

Bit 1

Position of axis 3

The angle at which the value of bit 1 changes depends on the particular robot type. The

following applies to robots whose axes 3 and 4 intersect:

= 0

A3 <0° (elbow down)

= 1

A3 ≥0° (elbow up)

Note:

For robots with an offset between axes 3 and 4, the

angle at which the value of bit 1 changes depends on

the magnitude of this offset.

Offset between A3 and A4

Bit 2

Position of axis 5

= 0

A5 ≥0° (no handflip)

= 1

A5 <0° (handflip)

Program example:

Program code

Comment

N14 T="T8MILLD20" D1

; $TC_DP3[1,1]=132.95

N16 ORIMKS

N17 G1 PTP X1665.67 Y0 Z1377.405 A=0 B=0 C=0 STAT=... F2000

; The STAT value defines

the articulated joint

positions (see below)

STAT=1 ('B001')

→ Shoulder left

→ Elbow down

→ No handflip

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

371

Transformations

7.10 Cartesian PTP travel

STAT=2 ('B010')

→ Shoulder right

→ Elbow up

→ No handflip

STAT=5 ('B101')

→ Shoulder left

→ Elbow down

→ Handflip

STAT=6 ('B110')

→ Shoulder right

→ Elbow up

→ Handflip

TRANSMIT

For TRANSMIT, the STAT address is used to initiate the equivocality regarding the pole.

Job Planning

372

Programming Manual, 12/2018, A5E40869460B AB

Transformations

7.10 Cartesian PTP travel

The following applies if the rotary axis must rotate through 180º or the contour for CP would

go through the pole:

Bit 0

Only relevant for $MC_TRANSMIT_POLE_SIDE_FIX_1/2 = 1 or 2:

= 0

Rotary axis traverses through +180º or rotates clockwise.

= 1

Rotary axis rotates through -180º or rotates counterclockwise.

Bit 1

Only relevant for $MC_TRANSMIT_POLE_SIDE_FIX_1/2 = 0:

= 0

The axis traverses through the pole. The rotary axis does not rotate.

= 1

The axis rotates around the pole. Bit 0 of STAT is relevant.

7.10.3

Specify the sign of the axis angle (TU)

In order that rotary axes can also approach axis angles exceeding +180° or less than -180°

without requiring a special traversing strategy (e.g. intermediate point), the sign of the axis

angle must be specified under the adjustable address TU.

Note

The control only takes into account programmed TU values for PTP motion. CP motion is

ignored.

Syntax

TU=<Value>

Meaning

TU:

Adjustable address to specify axis angle signs

<Value>:

Binary or decimal value

For each axis that is involved in the transformation, there is a bit that indicates the sign

of the axis angle (θ), and therefore the traversing direction.

Bit

= 0

Axis angle sign: +

Axis angular range: 0° ≤ θ < 360°

= 1

Axis angle sign: -

Axis angular range: - 360° < θ < 0°

Example: 6-axis articulated robot

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

373

Transformations

7.10 Cartesian PTP travel

$

$

$

$

$

$

Bit

Meaning

Value

Axis angle

Axis angle

sign

Bit 0 ¹⁾

Sign for the axis angle of A1

= 0

+

≥ 0°

= 1

-

< 0°

Bit 1 ¹⁾

Sign for the axis angle of A2

= 0

+

≥ 0°

= 1

-

< 0°

Bit 2 ¹⁾

Sign for the axis angle of A3

= 0

+

≥ 0°

= 1

-

< 0°

Bit 3 ¹⁾

Sign for the axis angle of A4

= 0

+

≥ 0°

= 1

-

< 0°

Bit 4 ¹⁾

Sign for the axis angle of A5

= 0

+

≥ 0°

= 1

-

< 0°

Bit 5 ¹⁾

Sign for the axis angle of A6

= 0

+

≥ 0°

= 1

-

< 0°

1)

The actual TU bit numbers obtained from the channel axis numbers of the robot axes! In the example,

robot axes (A1 to A6) are the first six axes in the channel; as a consequence, TU bits 0 ... 5 are used.

For another channel axis assignment of the robot axes, the TU bit numbers of the robot axes would

correspondingly change (e.g.: robot axes are the 3rd to 8th channel axis, i.e. TU bits 2 ... 7 are used

for the robot axes).

TU=19 (corresponds to TU='B010011) would therefore signify:

Bit

Value

Axis angle

0

= 1

①

θ_A1 < 0°

1

= 1

①

θ_A2 < 0°

Job Planning

374

Programming Manual, 12/2018, A5E40869460B AB

Transformations

7.10 Cartesian PTP travel

2

= 0

①

θ_A3 ≥ 0°

3

= 0

①

θ_A4 ≥ 0°

4

= 1

①

θ_A5 < 0°

5

= 0

①

θ_A6 ≥ 0°

Note

In the case of axes with a traversing range > ±360°, the axis always moves along the shortest

path because the axis position cannot be specified uniquely by the TU information.

If no TU is programmed for a position, then depending on MD30455

$MA_MISC_FUNCTION_MASK, the shorter or longer path is traversed (see Chapter "Taking

into account the software limits for PTP travel" in the Extended Functions Function Manual).

TRANSMIT

For PTP travel with TRANSMIT active, the address of TU has no meaning!

Example

The rotary axis position shown in the following diagram can be approached in the negative or

positive direction. The angular position is programmed under address A1. The traversing

direction is only absolutely clear when TU is specified.

6WDUWLQJ SRVLWLRQ

1HJDWLYH GLUHFWLRQ

$

r 78 ELW

3RVLWLYH GLUHFWLRQ

$

r 78 ELW

7DUJHW SRVLWLRQ

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

375

Transformations

7.10 Cartesian PTP travel

7.10.4

Example 1: PTP travel of a 6-axis robot with ROBX transformation

In the following application example, Cartesian PTP travel and the associated NC commands

are shown in the form of an example.

Figure 7-3

6-axis articulated robot with milling spindle

N1 G90

N2 T=“T8MILLD20“ D1 M6

N3 TRAORI

;$P_UIFR[1]=CTRANS(X,1500,Y,0,Z,400):CROT(X,0,Y,0,Z,-90)

N4 G54

N5 M3 S20000

N6 ORIWKS

N7 ORIVIRT1

N8 CYCLE832(0.01,_FINISH,1)

;HOME

N9 TRAFOOF

N10 G0 RA1=0.0000 RA2=-90.0000 RA3=90.0000 A=0.0000 B=90.0000 C=0.0000

N11 TRAORI

N12 G54

N13 G0 PTP X1369.2426 Y956.7528 Z502.5517 A=135.5761 B=-33.2223 C=161.1435

STAT='B010' TU='B001011'

N14 G0 X1355.1242 Y1014.9394 Z424.9695 A=135.8491 B=-33.1439 C=160.9941

STAT='B010' TU='B001011'

N15 G1 CP X1354.8361 Y1016.1269 Z423.3862 A=136.0635 B=-33.0819 C=160.8770

F1000

N16 G1 X1336.4283 Y1016.1269 Z426.6311 A=136.0484 B=-32.2151 C=160.9643

F2000

N17 G1 X1317.9831 Y1016.1269 Z429.6730 A=136.0175 B=-31.3394 C=161.0655

;HOME

N18 TRAFOOF

N19 G0 RA1=0.0000 RA2=-90.0000 RA3=90.0000 A=0.0000 B=90.0000 C=0.0000

N20 M30

Job Planning

376

Programming Manual, 12/2018, A5E40869460B AB

Transformations

7.10 Cartesian PTP travel

7.10.5

Example 2: PTP travel for generic 5-axis transformation

Assumption: Right-angled CA kinematics used as basis.

Program code

Comment

TRAORI

;Transformation CA kinematics ON

PTP

; Activate PTP traversal

N10 A3=0 B3=0 C3=1

; rotary axis positions C=0 A=0

N20 A3=1 B3=0 C3=1

; rotary axis positions C=90 A=45

N30 A3=1 B3=0 C3=0

; rotary axis positions C=90 A=90

N40 A3=1 B3=0 C3=1 STAT=1

; rotary axis positions C=270 A=-45

Select clear approach position of rotary axis position:

In block N40, the rotary axes - as a result of the programming of STAT=1 - travel the longer

distance from their start point (C=90, A=90) to the end point (C=270, A=-45). On the other

hand, with STAT=0, the rotary axes would travel along the shortest path to the end point (C=90,

A=45).

7.10.6

Example 3: PTPG0 and TRANSMIT

Traversing around the pole with PTPG0 and TRANSMIT

<

PTP

CP

1

* ;

<

1

;

<

;

Program code

Comment

N001 G0 X30 Z0 F10000 T1 D1 G90

;Initial setting absolute dimension

N002 SPOS=0

N003 TRANSMIT

;TRANSMIT transformation

N010 PTPG0

; for each G0 block, automatically PTP -

and then CP again.

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

377

Transformations

7.10 Cartesian PTP travel

Program code

Comment

N020 G0 X30 Y20

N030 X-30 Y-20

N120 G1 X30 Y20

N110 X30 Y0

M30

Traversing from the pole with PTPG0 and TRANSMIT

<

PTP

CP

30

N070 X20 Y2

20

10

N060 X0 Y0

-30

-20

-10

10

20

30

;

-10

-20

-30

N050 X10 Y0

Programming

Comment

N001 G0 X90 Z0 F10000 T1 D1 G90

;Initial setting

N002 SPOS=0

N003 TRANSMIT

;TRANSMIT transformation

N010 PTPG0

; for each G0 block, automatically PTP -

and then CP again.

N020 G0 X90 Y60

N030 X-90 Y-60

N040 X-30 Y-20

N050 X10 Y0

N060 X0 Y0

N070 X-20 Y2

N170 G1 X0 Y0

N160 X10 Y0

N150 X-30 Y-20

M30

Job Planning

378

Programming Manual, 12/2018, A5E40869460B AB

Kinematic chains

8.1 Deletion of components (DELOBJ)

Meaning

DELOBJ:

Deletion of elements from kinematic chains, protection areas, protection area ele-

ments, collision pairs and transformation data

<CompType>:

Component type to be deleted

Data type:

STRING

Value: "KIN_CHAIN_ELEM"

Meaning: System variables of all kinematic elements: $NK_...

Value: "KIN_CHAIN_SWITCH"

Meaning: System variable $NK_SWITCH[<i>]

Value: "KIN_CHAIN_ALL"

Meaning: All kinematic elements and switches.

Is the same as the successive call of DELOBJ with "KIN_CHAIN_ELEM" and

"KIN_CHAIN_SWITCH"

Value: "PROT_AREA"

Meaning: System variables of the protection areas:

● $NP_PROT_NAME

● $NP_CHAIN_NAME

● $NP_CHAIN_ELEM

● $NP_1ST_PROT

Value: "PROT_AREA_ELEM"

Meaning: System variables of the protection area elements of machine protection

areas and/or automatic tool protection areas:

● $NP_NAME

● $NP_NEXT

● $NP_NEXTP

● $NP_COLOR

● $NP_D_LEVEL

● $NP_USAGE

● $NP_TYPE

● $NP_FILENAME

● $NP_PARA

● $NP_OFF

● $NP_DIR

● $NP_ANG

Value: "PROT_AREA_COLL_PAIRS"

Meaning: System variables of the collision pairs:

● $NP_COLL_PAIR

● $NP_SAFETY_DIST

Value: "PROT_AREA_ALL"

Meaning: All protection areas, protection area elements and collision pairs (system

variable $NP_... )

Is the same as the successive call of DELOBJ with "PROT_AREA,"

"PROT_AREA_ELEM," and "PROT_AREA_COLL_PAIRS"

Value: "TRAFO_DATA"

Meaning: System variables of all transformations $NT_...

Job Planning

382

Programming Manual, 12/2018, A5E40869460B AB

Kinematic chains

8.1 Deletion of components (DELOBJ)

<Index1>:

Index of the first component to be deleted (optional)

Data type:

INT

Default value:

-1

Range of val-

-1 ≤ x ≤ (maximum number of configured components -1)

ues:

Value

Meaning

0, 1, 2,

Index of the component to be deleted.

-1

All components of the specified type are deleted. <Index2> is not

evaluated.

<Index2>:

Index of the last components to be deleted (optional)

If <Index2> is not programmed, only the system variables of the component refer-

enced in <Index1> are deleted.

Data type:

INT

Default value:

Only the system variables of the component referenced in <In-

dex1> are deleted.

Range of val-

<Index1> < x ≤ (max. number of configured components -1)

ues:

<NoAlarm>:

Alarm suppression (optional)

Data type:

BOOL

Default value:

FALSE

Value

Meaning

FALSE

In the event of an error (<RetVal> < 0), program processing is

stopped and an alarm displayed.

TRUE

In the event of an error, the program processing is not stopped

and no alarm displayed.

Application: User-specific reaction corresponding to the return

value

<RetVal>:

Function return value

Data type:

INT

Range of val-

0, -1, -2, ... -7

ues:

Value

Meaning

0

No error occurred.

-1

Call of the function without parameters. At least parameter

<CompType> must be specified.

-2

<CompType> identifies an unknown component

-3

<Index1> is less than -1

-4

<Index1> is greater than the configured number of components

-5

<Index1> has a value not equal to -1 when deleting a component

group

-6

<Index2> is less than <Index1>

-7

<Index2> is greater than the configured number of components

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

383

Kinematic chains

8.2 Index determination by means of names (NAMETOINT)

8.2

Index determination by means of names (NAMETOINT)

User-specific names are entered in the system variable arrays of type STRING. Based on the

identifier of the system variables and the name, the NAMETOINT() function determines the

index value belonging to the name under which it is stored in the system variable array.

Syntax

<RetVal> = NAMETOINT(<SysVar>,<Name>[,<NoAlarm>])

Meaning

NAMETOINT:

Determining the system variable index

<SysVar>:

Name of the system variable array of typeSTRING

Data type:

STRING

Range of val-

Name of all NC system variable arrays of type STRING

ues:

<Name>:

Character string or name for which the system variable index is to be determined.

Data type:

STRING

<NoAlarm>:

Alarm suppression (optional)

Data type:

BOOL

Default value:

FALSE

Value

Meaning

TRUE

In the event of an error, the program processing is not stopped

and no alarm displayed.

Application: User-specific reaction corresponding to the return

value

FALSE

In the event of an error (<RetVal> < 0), program processing is

stopped and an alarm displayed.

<RetVal>:

System variable index or error message

Data type:

INT

Range of val-

-1 ≤ x ≤ (max. number of configured components -1)

ues:

Value

Meaning

≥ 0

The sought name has been found under the specified system

variable index.

-1

The sought name has not been found or an error has occurred.

Example

Program code

Comment

DEF INT INDEX

$NP_PROT_NAME[27]="Cover"

INDEX = NAMETOINT("$NP_PROT_NAME","Cover")

; INDEX == 27

Job Planning

384

Programming Manual, 12/2018, A5E40869460B AB

Collision avoidance with kinematic chains

9.1 Check for collision pair (COLLPAIR)

9.1

Check for collision pair (COLLPAIR)

The COLLPAIR() function determines whether two protection areas form a collision pair.

Syntax

[<RetVal> =] COLLPAIR(<Name_1>,<Name_2>[,<NoAlarm>)])

Meaning

COLLPAIR:

Check whether part of a collision pair

<RetVal>:

Function return value

Data type:

INT

Value:

≥ 0

The two protection zones form a collision pair.

Return value == collision pair index m (see

$NP_COLL_PAIR)

-1

Either two strings have not been specified or at least

one of the two is the zero string.

-2

The protection zone specified in the first parameter has

not been found.

-3

The protection zone specified in the second parameter

has not been found.

-4

Neither of the two specified protection zones has been

found.

-5

Both specified protection zones have been found, but

not together in a collision pair.

<Name_1>:

Name of the first protection zone

Data type:

STRING

Range of val-

Parameterized protection zone names

ues:

<Name_2>:

Name of the second protection area

Data type:

STRING

Range of val-

Parameterized protection zone names

ues:

<NoAlarm>:

Alarm suppression (optional)

Data type:

BOOL

Value:

FALSE (Default)

In the event of an error (<RetVal> < 0), the

program processing is stopped and an alarm

displayed.

TRUE

In the event of an error, the program process-

ing is not stopped and no alarm displayed.

Application: User-specific reaction corre-

sponding to the return value

Job Planning

386

Programming Manual, 12/2018, A5E40869460B AB

Collision avoidance with kinematic chains

9.2 Request recalculation of the machine model of the collision avoidance (PROTA)

9.2

Request recalculation of the machine model of the collision avoidance

(PROTA)

If system variables of the kinematic chain $NK_..., the geometric machine modeling or the

collision avoidance $NP_... are written in the part program, the PROTA procedure must

subsequently be called so that the change becomes effective in the NC-internal machine model

of the collision avoidance.

Syntax

PROTA[(<Par>)]

Meaning

PROTA:

Request recalculation of the machine model of the collision avoidance

● Triggers a preprocessing stop.

● Must be alone in the block.

<Par>:

Parameter (optional)

Data type:

STRING

Value:

---

No parameters.

The machine model is recalculated. The states of the pro-

tection areas are retained.

"R"

The machine model is recalculated. The protection areas

are set to their initialization status corresponding to

$NP_INIT_STAT.

Supplementary conditions

Simulation

The PROTA procedure must not be used in part programs in conjunction with the simulation

(simNC).

Example: Avoiding the PROTA call while the simulation is active.

Program code

Comment

IF $P_SIM == FALSE

; IF simulation not active

PROTA

THEN recalculate collision model

ENDIF

; ENDIF

See also

Setting the protection zone status (PROTS) (Page 388)

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

387

Collision avoidance with kinematic chains

9.3 Setting the protection zone status (PROTS)

9.3

Setting the protection zone status (PROTS)

The PROTS() procedure sets the state of protection areas to the specified value.

Syntax

PROTS(<State>[,<Name_1>,...,<Name_n>])

Meaning

PROTS:

Sets the state of protection areas

● Must be alone in the block.

<State>:

Status to which the specified protection zones are to be set

Data type:

CHAR

Value:

"A"or "a"

Status: Active

"I"or "i"

Status: Inactive

"P"or "p"

Status: Preactivated or PLC-controlled ¹⁾

"R"or "r"

Status: NC-internal value of the initialization

status ²⁾

<Name_1> ...

Name of one or more protection areas that are to be set to the specified status

<Name_n>:

(optional)

If no name is specified, the specified status is set for all defined protection zones.

Data type:

STRING

Range of values:

Parameterized protection zone names

Note

The maximum number of protection areas that can be specified as parameters

depends only on the maximum possible number of characters per program line.

¹⁾ The activation/deactivation is performed via: DB10.DBX234.0 - DBX241.7

²⁾ The status is set to the NC-internal value of the initialization status, i.e. to the value that the system

variable $NP_INIT_STAT had at the time of the last PROTA( ) (Page 387) call.

Job Planning

388

Programming Manual, 12/2018, A5E40869460B AB

Collision avoidance with kinematic chains

9.4 Determining the clearance of two protection zones (PROTD)

9.4

Determining the clearance of two protection zones (PROTD)

The PROTD() function calculates the clearance of two protection areas.

Function properties:

● The clearance calculation is performed independent of the protection area status (activated,

deactivated, preactivated).

● To calculate the clearance of two protection areas, only protection area elements are used,

which are marked with $NP_USAGE = "C" or "A". Protection area elements of the protection

area, which are marked with $NP_USAGE = "V", are not taken into consideration.

● Protection areas, where all protection area elements of the protection area are marked with

$NP_USAGE = "V", cannot be used for the clearance calculation.

● The clearance calculation is performed with the positions valid at the end of the previous

block.

● Overlays that are included in the main run calculation (e.g. DRF offset or external zero

offset) are included in the clearance calculation with the values valid at the function

interpretation time.

Note

Synchronization

When using the PROTD() function, it is the sole responsibility of the user to synchronize

the main run and preprocessing, if required, with the STOPRE preprocessing stop.

Collision

If there is a collision between the specified protection areas, the function returns a clearance

of 0.0. There is a collision if both the protection areas touch or intersect each other.

The safety clearance for the collision check (MD10622 $MN_COLLISION_SAFETY_DIST) is

not taken into account in the clearance calculation.

Syntax

[<RetVal> =] PROTD([<Name_1>],[<Name_2>],VAR <Vector>[,<System>])

Meaning

PROTD:

Calculates the clearance of the two specified protection areas.

● Must be alone in the block.

<RetVal>:

Function return value: Absolute clearance value of the two protection areas or 0.0

with collision (see above: Collision paragraph)

Data type:

REAL

Range of values:

0.0 ≤ x ≤ +max. REAL value

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

389

Collision avoidance with kinematic chains

9.4 Determining the clearance of two protection zones (PROTD)

<Name_1>,

Names of the two protection areas whose clearance is to be calculated (optional)

<Name_2>:

Data type:

STRING

Range of values:

Parameterized protection area names

Default value:

"" (empty string)

If no protection areas have been specified, the function calcu-

lates the current smallest clearance from all the activated and

preactivated protection areas in the collision model.

<Vector>:

Return value: 3-dimensional clearance vector from protection area <Name_2> to

protection area <Name_1> with:

● <Vector>[0]: X coordinate in the world coordinate system

● <Vector>[1]: Y coordinate in the world coordinate system

● <Vector>[2]: Z coordinate in the world coordinate system

For collision: <Vector> == zero vector

Data type:

VAR REAL [3]

Range of values:

<Vector> [n]: 0.0 ≤ x ≤ ±max. REAL value

<System>:

Measuring system (inch/metric) for clearance and clearance vector (optional)

Data type:

BOOL

Value:

FALSE (Default)

Measuring system corresponding to the cur-

rently active G command from G group 13

(G70, G71, G700, G710).

TRUE

Measuring system corresponding to the set

basic system:

MD52806 $MN_ISO_SCALING_SYSTEM

Job Planning

390

Programming Manual, 12/2018, A5E40869460B AB

Transformation with kinematic chains

10

10.1

Activating a transformation (TRAFOON)

A transformation defined with kinematic chains is activated with the predefined TRAFOON

procedure. The call must be alone in a block.

Note

Alternatively, a transformation defined with kinematic chains can also be activated via

conventional NC commands, such as TRAORI or TRANSMIT. For this purpose, an appropriate

value, not equal to zero, must be entered in the $NT_TRAFO_INDEX system variable.

For further information on $NT_TRAFO_INDEX see "System Variables List Manual".

Syntax

TRAFOON(<Trafoname>,<Diameter>,<k>)

Meaning

TRAFOON:

Procedure for activating a transformation defined with kinematic chains

<Trafoname>:

Name of the transformation data set

Data type:

STRING

Range of val-

All names of transformation data sets defined via $NK_NAME

ues:

Note:

The name of the transformation data set must be unique. It must only occur once

in $NT_NAME.

<Diameter>:

Reference or working diameter (TRACYL only)

Data type:

REAL

The value must be > 1.

<k>:

Defines the use of the groove side offset (TRACYL only).

Data type:

BOOL

Value:

FALSE

Without groove side offset

TRUE

With groove side offset

Corresponds to the TRACYL transformation type 514 (groove side offset can be

programmed). If <k> is not specified, the parameterized setting of bit 10 in

$NT_CNTRL[<n>] applies.

Example

Program code

Comment

TRAFOON["Trans_1"]

Activates the transformation with the name Trans_1.

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

391

Transformation with kinematic chains

10.2 Modifying the orientation transformation after the machine measurement (CORRTRAFO)

10.2

Modifying the orientation transformation after the machine

measurement (CORRTRAFO)

For machines with orientation transformations that were defined by means of kinematic chains,

the user can use the predefined CORRTRAFO function in order to modify the offset vectors

or the direction vectors of the orientation axes in the kinematic model of the machine after a

machine measurement.

Syntax

<Corr_Status> = CORRTRAFO(<Corr_Vect>, <Corr_Index>, <Corr_Mode>,

[ <No_Alarm>])

Meaning

CORRTRAFO:

Function call

<Corr_Status>:

Function return value

Data type:

INT

Values:

0

The function was executed without an error.

1

No transformation is active.

2

The currently active transformation is not an orientation trans-

formation.

3

The active orientation transformation was not defined with kin-

ematic chains.

10

The <Corr_Index> call parameter is negative.

11

The <Corr_Mode> call parameter is negative.

12

Invalid reference to a section of a subchain (unit position of

<Corr_Index>). The value must not be greater than the num-

ber of orientation axes in the subchain.

13

Invalid reference to the orientation axis of a subchain (unit po-

sition of <Corr_Index>). The value must be less than the

number of orientation axes in the subchain.

14

Invalid reference to a subchain (tens position of

<Corr_Index>). Only the values 0 and 1 are permissible (ref-

erence to part or tool chain). This error number occurs if the

subchain to which <Corr_Index> refers does not exist.

Job Planning

392

Programming Manual, 12/2018, A5E40869460B AB

Transformation with kinematic chains

10.2 Modifying the orientation transformation after the machine measurement (CORRTRAFO)

15

There is no correction element in the section referred to with

the <Corr_Index> parameter ($NT_CORR_ELEM_P or

$NT_CORR_ELEM_T).

20

Invalid correction mode (unit position of <Corr_Mode>). Only

the values 0 and 1 are permissible.

21

Invalid correction mode (tens and/or hundreds position of

<Corr_Mode>). Only the unit position can be not equal to zero

when writing an axis direction.

30

The hundreds position of <Corr_Mode> is invalid. Only the

values 0 and 1 are permissible.

31

The thousands position of <Corr_Mode> is invalid. Only the

values 0 and 1 are permissible.

40

The direction vector that is to be taken as axis direction is the

zero vector. This error can only happen if the thousands posi-

tion of <Corr_Mode> is equal to 0. If the thousands position

of this parameter is equal to 1 (monitoring of the maximum

correction deactivated), the zero vector can also be written.

41

For the correction of an offset vector, the difference to the cur-

rent value in at least one coordinate is greater than the maxi-

mum value specified by the setting data SD41610

$SN_CORR_TRAFO_LIN_MAX. The <Corr_Vect> parame-

ter will be overwritten by an error vector. This also applies when

the processing is aborted with alarm (see <No_Alarm> pa-

rameter).

In the components whose correction value has exceeded the

permissible limit, the error vector has the difference, with the

correct sign, between the determined correction value and the

limit.

The content of the components that have not exceeded their

limit is zero.

42

For the correction of a direction vector, the angular displace-

ment compared to the current direction is greater than the

maximum value specified by the setting data SD41611

$SN_CORR_TRAFO_DIR_MAX.

43

The attempt to write a system variable was rejected because

of missing write rights.

<Corr_Vect>:

Correction vector

The content of the correction vector is defined by the following parameters

<Corr_Index> and <Corr_Mode>.

If <Corr_Status> = 41, the content of the vector is overwritten (see above).

Data type:

REAL

<Corr_Index>:

Section whose correction element is to be modified /

index of the orientation axis whose direction vector is to be modified

Data type:

INT

The <Corr_Index> parameter is decimal coded (unit to tens position):

Unit

Contains the index of the section or the orientation axis in the sub-

position:

chain.

Tens

Refers to the subchain.

position:

0x

Workpiece chain

1x

Tool chain

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

393

Transformation with kinematic chains

10.2 Modifying the orientation transformation after the machine measurement (CORRTRAFO)

<Corr_Mode>:

Correction mode

Data type:

INT

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

Unit

Specifies which element is to be corrected.

position:

xxx0

Correction of a linear offset vector

xxx1

Correction of the direction vector of an orientation axis

Tens

Specifies how the correction element to which the content of

position:

<Corr_Index> refers, is to be modified.

xx0x

The correction vector is written immediately to the correc-

tion element.

This variant can be used to immediately write the correction

element without the index <n> of the relevant system data

($NK_OFF_DIR[<n>, ...]) having to be known.

xx1x

As 0, but with the difference that the transferred correction

value is interpreted in world coordinates.

A difference between variants 0 and 1 can always occur

when the kinematic chain in the initial state (positions of all

orientation axes equal to 0) contains other rotations.

xx2x

As 1, but with the difference that the correction value refers

to the entire section, i.e. a value is entered in the correction

element so that the entire section reaches the length de-

fined by the correction value.

Note:

The values 1 and 2 are not permissible when writing the direction

vector of an orientation axis.

Hundreds

Specifies how the content of the <Corr_Vect> parameter is to be

position:

interpreted.

x0xx

The transferred correction vector <Corr_Vect> contains

the entire new length of the correction element or the sec-

tion to which the <Corr_Index> in conjunction with the

tens position of <Corr_Mode> refers (absolute correction).

x1xx

The transferred correction vector <Corr_Vect> only con-

tains the difference compared to the current length of the

correction element or the section to which the

<Corr_Index> in conjunction with the tens position of

<Corr_Mode> refers (incremental correction).

Note:

For the correction of the direction vector of an orientation axis, the

content of the hundreds position must be 0.

Thou-

Specifies whether the correction is to be limited by the following

sands

maximum value:

position:

● SD41610 $SN_CORR_TRAFO_LIN_MAX

or

● SD41611 $SN_CORR_TRAFO_DIR_MAX

0xxx

Monitoring of the maximum correction is active.

1xxx

Monitoring of the maximum correction is not active.

Job Planning

394

Programming Manual, 12/2018, A5E40869460B AB

Transformation with kinematic chains

10.2 Modifying the orientation transformation after the machine measurement (CORRTRAFO)

<No_Alarm>:

Behavior in the event of an error (return value > 0) (optional)

Data type:

BOOL

Value:

FALSE

In the event of an error, the program processing is stop-

(default)

ped and alarm 14103 is displayed.

TRUE

In the event of an error, the program processing is not

stopped and no alarm is displayed.

Application: User-specific reaction corresponding to the

return value

Note

In the event of an error when the function is called, either an alarm is output or an error number

returned (see <No_Alarm> parameter), so that the user can respond in a suitable way to the

error state. The cause of the error is described in more detail through an alarm parameter. An

error number returned instead of an alarm is identical to the alarm parameter.

Further information on CORRTRAFO

The kinematic structure of a machine with orientation transformation is described by one or

two kinematic chains (subchains), starting from the zero point of the world coordinate system.

One of the two chains, the tool chain, ends at the reference point of the tool, the other chain,

the workpiece chain ends in the zero point of the basic coordinate system.

The CORRTRAFO function writes lever arm lengths and axis directions on machines with an

orientation transformation in special correction elements. A kinematic chain is described, for

example, with elements of the type OFFSET, which are defined via $ NK_TYPE.

CORRTRAFO works with sections

The two subchains can each be divided into a maximum of four sections:

● Section 1 begins at the starting point of the chain and ends at the first orientation axis.

● Section 2 is the section between orientation axis 1 and orientation axis 2.

● Section 3 is the section between orientation axis 2 and orientation axis 3.

● Section 4 is the section between orientation axis 3 and the end of the tool or workpiece

chain.

Each section may contain constant chain elements of the type OFFSET or ROT_CONST.

The following figure shows an orientation transformation with 2 orientation axes.

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

395

Transformation with kinematic chains

10.2 Modifying the orientation transformation after the machine measurement (CORRTRAFO)

2ULHQWDWLRQ D[LV

6HFWLRQ

,QGH[

2ULHQWDWLRQ D[LV

6HFWLRQ

,QGH[

6HFWLRQ

,QGH[

7RRO UHIHUHQFH SRLQW HQG

SRLQW RI WKH WRRO FKDLQ

:RUNSLHFH UHIHUHQFH

SRLQW

7DEOH RIIVHW

=HUR SRLQW RI WKH ZRUOG

FRRUGLQDWH V\VWHP

Figure 10-1

CORRTRAFO example

The sections are clearly defined: If you run through the kinematic subchain from the starting

point to the end point, the first section has the index 0, the next the index 1, and so on. The

index of the last section is then always equal to the number of orientation axes.

Correction elements

A reference can be made to a constant kinematic chain element (chain element of the type

$NK_TYPE[<n>] = "OFFSET") in each section with the $NT_CORR_ELEM_T[<n>, 0 ... 3] or

$NT_CORR_ELEM_P[<n>, 0 ... 3] system variables. The correction values that were

determined during the machine measurement are written to these elements with the

CORRTRAFO function.

Example with transformation index = 1:

● $NT_CORR_ELEM_T[1,0] = "C_AXIS_OFFSET"; Offset of the C axis (orientation axis 1)

in section 1 is defined as correction element.

● $NT_CORR_ELEM_T[1,1] = "B_AXIS_OFFSET"; Offset of the B axis (orientation axis 2) in

section 2 is defined as correction element.

● $NT_CORR_ELEM_T[1,2] = "BASE_TOOL_OFFSET"; Offset of the B axis from the tool

reference point in section 3 is defined as correction element.

The sequence of the references in $NT_CORR_ELEM_T/P[<n>, 0 ... 3] must correspond to

the sections described above, i.e. only one chain element can be in $NT_CORR_ELEM_T/P

[<n>, 0] which is before the first orientation axis, etc.

The CORRTRAFO function writes the values determined by measuring the machine into the

correction elements defined in this way. The modification of the correction values is defined

in CORRTRAFO via the <Corr_Mode> parameter.

Job Planning

396

Programming Manual, 12/2018, A5E40869460B AB

Tool offsets

11

11.1

Offset memory

Structure of the offset memory

Every data field can be called with a T and D number, and contains not only the geometric

specifications for the tool but also further entries, such as the tool type.

User cutting edge data

User cutting edge data can be configured via machine data. Please refer to the machine

manufacturer's instructions.

Tool parameters

Note

Individual values in the offset memory

The individual values of the offset memory P1 to P25 can be read and written by the program

via system variables. All other parameters are reserved.

The tool parameters $TC_DP6 to $TC_DP8, $TC_DP10 and $TC_DP11 as well as $TC_DP15

to $TC_DP17, $TC_DP19 and $TC_DP20 have another meaning depending on tool type.

Tool parameter number (DP) Meaning of system variables

Remark

$TC_DP1

Tool type

For overview see list

$TC_DP2

Cutting edge position

Only for turning tools

Geometry

Length compensation

$TC_DP3

Length 1

Allocation to

$TC_DP4

Length 2

Type and level

$TC_DP5

Length 3

Geometry

Radius

$TC_DP6 ¹⁾

Radius 1 / length 1

Milling/turning/grinding tool

$TC_DP6 ²⁾

diameter d

Slotting saw

$TC_DP7 ¹⁾

Length 2 / corner radius, tapered milling tool

Milling tools

$TC_DP7 ²⁾

Slot width b corner radius

Slotting saw

$TC_DP8 ¹⁾

Rounding radius 1 for milling tools

Milling tools

$TC_DP8 ²⁾

projecting length k

Slotting saw

$TC_DP9 ^{1) 3)}

Rounding radius 2

Reserved

$TC_DP10 ¹⁾

Angle 1 face end of tool

Tapered milling tools

$TC_DP11 ¹⁾

Angle 2 tool longitudinal axis

Tapered milling tools

Wear

Length and radius compensation

$TC_DP12

Length 1

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

399

Tool offsets

11.1 Offset memory

Tool parameter number

Meaning

Cutting Dn

Remark

(DP)

$TC_DP4

Length 2

$TC_DP5

Length 3

Geometry

Radius

$TC_DP6

Radius

Geometry

Limit angle

$TC_DP10

Minimum limit angle

$TC_DP11

Maximum limit angle

Wear

Length and radius compensation

$TC_DP12

Wear length 1

$TC_DP13

Wear length 2

$TC_DP14

Wear length 3

$TC_DP15

Wear radius

Wear

Limit angle

$TC_DP19

Wear min. limit angle

$TC_DP20

Wear max. limit angle

Tool base dimension/

Length offsets

adapter

$TC_DP21

Length 1

$TC_DP22

Length 2

$TC_DP23

Length 3

Basic value and wear value

The resultant values are each a total of the basic value and wear value (e.g. $TC_DP6 +

$TC_DP15 for the radius). The basic measurement ($TC_DP21 - $TC_DP23) is also added

to the tool length of the first cutting edge. All the other parameters, which may also impact on

effective tool length for a standard tool, also affect this tool length (adapter, orientational

toolholder, setting data).

Limit angles 1 and 2

Limit angles 1 and 2 each relate to the vector of the cutting edge center point to the cutting

edge reference point and are counted clockwise.

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

401

Tool offsets

11.2 Additive offsets

Example

The same cutting edge is used for two bearing seats:

/RFDWLRQ RI XVH

/RFDWLRQ RI XVH

;

' '/

'

=

Program code

Comment

N110 T7 D7

; The revolver is positioned to location 7. D7 and DL=1

are activated and moved through in the next block.

N120 G0 X10 Z1

N130 G1 Z-6

N140 G0 DL=2 Z-14

; DL=2 is activated in addition to D7 and is moved through

in the next block.

N150 G1 Z-21

N160 G0 X200 Z200

; Approach tool change point.

11.2.2

Specify wear and setup values ($TC_SCPxy[t,d], $TC_ECPxy[t,d])

Wear and setting-up values can be read and written to using system variables. The logic is

based on the logic of the corresponding system variables for tools and tool noses.

System variables

$TC_SCPxy[<t>,<d>]:

Wear values that are assigned to the particular geometry parameters

via xy, whereby x corresponds to the number of the wear value and y

establishes the reference to the geometry parameter.

$TC_ECPxy[<t>,<d>]:

Setting-up values that are assigned to the particular geometry param-

eter via xy, whereby x corresponds to the number of the setting-up

value and y establishes the reference to the geometry parameter.

<t>: T number of the tool

<d>: D number of the tool cutting edge

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

403

Tool offsets

11.2 Additive offsets

Note

The defined wear and setup values are added to the geometry parameters and the other offset

parameters (D numbers).

Example

The wear value of length 1 is set to the value of 1.0 for the cutting edge <d> of tool <t>.

Parameter: $TC_DP3 (length 1, with turning tools)

Wear values: $TC_SCP13 to $TC_SCP63

Setup values: $TC_ECP13 to $TC_ECP63

$TC_SCP43 [<t>,<d>] = 1.0

11.2.3

Delete additive offsets (DELDL)

The DELDL command deletes the additive offsets for the cutting edge of a tool (to release

memory space). Both the defined wear values and the setup values are deleted.

Syntax

DELDL[<t>,<d>]

DELDL[<t>]

DELDL

<Status>=DELDL[<t>,<d>]

Meaning

DELDL:

Command to delete additive offsets

<t>:

T number of the tool

<d>:

D number of the tool cutting edge

DELDL[<t>,<d>]:

All additive offsets of the cutting edges <d> of the tool <t> are deleted.

DELDL[<t>]:

All additive offsets of all cutting edges of tool <t> are deleted.

DELDL:

All additive offsets of all cutting edges of all tools of the TO unit are deleted

(for the channel in which the command is programmed).

<Status>:

Delete status

Value:

Meaning:

0

Deletion was successfully completed.

-

Offsets have not been deleted (if the parameter settings specify ex-

actly one tool edge), or not deleted completely (if the parameter

settings specify several cutting edges).

Job Planning

404

Programming Manual, 12/2018, A5E40869460B AB

Tool offsets

11.3 Special handling of tool offsets

11.3

Special handling of tool offsets

The evaluation of the sign for tool length and wear can be controlled using setting data

SD42900 to SD42960.

The same applies to the behavior of the wear components when mirroring geometry axes or

changing the machining plane, and also to temperature compensation in tool direction.

Wear values:

If reference is made to wear values in the following, then this should be understood as the sum

of the actual wear values ($TC_DP12 to $TC_DP20) and the sum offsets with the wear values

($SCPX3 to $SCPX11) and setting-up values ($ECPX3 to $ECPX11).

For more information about summed offsets, refer to:

References:

Function Manual, Tool Management

Setting data

SD42900 $SC_MIRROR_TOOL_LENGTH

Mirroring of tool-length components and compo-

nents of the tool base dimension.

SD42910 $SC_MIRROR_TOOL_WEAR

Mirroring of wear values of the tool-length compo-

nents.

SD42920 $SC_WEAR_SIGN_CUTPOS

Evaluating the sign of the wear components as a

function of the cutting edge position.

SD42930 $SC_WEAR_SIGN

Inverts the sign of wear dimensions.

SD42935 $SC_WEAR_TRANSFORM

Transformation of wear values.

SD42940 $SC_TOOL_LENGTH_CONST

Assignment of tool length components to geome-

try axes.

SD42950 $SC_TOOL_LENGTH_TYPE

Assignment of the tool length components inde-

pendent of tool type.

SD42960 $SC_TOOL_TEMP_COMP

Temperature compensation value in tool direction.

Also operative when tool orientation is program-

med.

References

Function Manual Basic Functions; Tool Offset (W1)

Further information

Activation of modified setting data

When the setting data described above is modified, the tool components are not reevaluated

until the next time a tool edge is selected. If a tool is already active and the data of this tool is

to be reevaluated, the tool must be selected again.

Job Planning

406

Programming Manual, 12/2018, A5E40869460B AB

Tool offsets

11.3 Special handling of tool offsets

The same applies in the event that the resulting tool length is modified due to a change in the

mirroring status of an axis. The tool must be selected again after the mirror command, in order

to activate the modified tool-length components.

Orientable toolholders and new setting data

Setting data SD42900 to SD42940 has no effect on the components of an active toolholder

with orientation capability. However, the calculation with an orientable toolholder always allows

for a tool with its total resulting length (tool length + wear + tool base dimension). All

modifications initiated by the setting data are included in the calculation of the resulting total

length, i.e. vectors of the orientable toolholder are independent of the machining plane.

Note

When orientable toolholders are used, it is frequently practical to define all tools for a non-

mirrored basic system, even those which are only used for mirrored machining. When

machining with mirrored axes, the toolholder is then rotated such that the actual position of

the tool is described correctly. All tool-length components then automatically act in the correct

direction, dispensing with the need for control of individual component evaluation via setting

data, depending on the mirroring status of individual axes.

Further application options

The use of orientable toolholder functionality can also be useful if there is no physical option

of turning tools on the machine, even though tools with different orientations are permanently

installed. Tool dimensioning can then be performed uniformly in a basic orientation, where the

dimensions relevant for machining are calculated according to the rotations of a virtual

toolholder.

11.3.1

Mirroring of tool lengths

When setting data SD42900 $SC_MIRROR_TOOL_LENGTH and

SD42910 $SC_MIRROR_TOOL_WEAR are not set to zero, then you can mirror the tool length

components and components of the basis dimensions with wear values and their associated

axes.

;

'

;

=

=

0

:

:

0

:&6

:&6

' ZLWK 6/

' ZLWK 6/

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

407

Tool offsets

11.3 Special handling of tool offsets

SD42900 $SC_MIRROR_TOOL_LENGTH

Setting data not equal to zero:

The tool length components ($TC_DP3, $TC_DP4 and $TC_DP5) and the components of the

basis dimensions ($TC_DP21, $TC_DP22 and $TC_DP23) are mirrored against their

associated axes, also mirrored - by inverting the sign.

The wear values are not mirrored. If these are also be be mirrored, then setting data

SD42910 $SC_MIRROR_TOOL_WEAR must be set.

SD42910 $SC_MIRROR_TOOL_WEAR

Setting data not equal to zero:

The wear values of the tool length components - whose associated axes are mirrored - are

also mirrored by inverting the sign.

11.3.2

Wear sign evaluation

When setting data SD42920 $SC_WEAR_SIGN_CUTPOS and SD42930 $SC_WEAR_SIGN

are set not equal to zero, then you can invert the sign evaluation of the wear components.

SD42920 $SC_WEAR_SIGN_CUTPOS

Setting data not equal to zero:

For tools with the relevant cutting edge position (turning and grinding tools, tool types 400),

then the sign evaluation of the wear components in the machining plane depends on the cutting

edge position. This setting data is of no significance for tool types without relevant cutting edge

position.

In the following table, the dimensions, whose sign is inverted using SD42920 (not equal to

zero), are designed using an X:

Cutting edge position

Length 1

Length 2

1

2

X

3

X

X

4

X

5

6

7

X

8

X

9

Note

The sign evaluation using SD42920 and SD42910 are independent of one another. If, for

example, the sign of a dimension is changed using both setting data, then the resulting sign

remains unchanged.

Job Planning

408

Programming Manual, 12/2018, A5E40869460B AB

Tool offsets

11.3 Special handling of tool offsets

SD42930 $SC_WEAR_SIGN

Setting data not equal to zero:

Inverts the sign of all wear dimensions. This affects both the tool length and other variables

such as tool radius, rounding radius, etc.

If a positive wear dimension is entered, the tool becomes "shorter" and "thinner", refer to

Chapter "tool offset, special handling", activating changed setting data".

11.3.3

Coordinate system of the active machining operation (TOWSTD, TOWMCS,

TOWWCS, TOWBCS, TOWTCS, TOWKCS)

Depending on the kinematics of the machine or the availability of an orientable tool carrier, the

wear values measured in one of these coordinate systems are converted or transformed to a

suitable coordinate system.

Coordinate systems of active machining operation

The following coordinate systems produce tool length offsets which the tool length wear

component incorporates in an active tool via the corresponding G command of Group 56:

● Machine coordinate system (MCS)

● Basic coordinate system (BCS)

● Workpiece coordinate system (WCS)

● Tool coordinate system (TCS)

● Tool coordinate system of kinematic transformation (KCS)

Syntax

TOWSTD

TOWMCS

TOWWCS

TOWBCS

TOWTCS

TOWKCS

Meaning

TOWSTD:

Initial setting value for offsets in tool length wear value

TOWMCS:

Offsets in tool length in MCS

TOWWCS:

Offsets in tool length in WCS

TOWBCS:

Offsets in tool length in BCS

TOWTCS:

Offsets in tool length at tool carrier reference point (orientable tool carrier)

TOWKCS:

Compensations of tool length for tool head (kinematic transformation)

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

409

Tool offsets

11.3 Special handling of tool offsets

Further information

Distinguishing features

The most important distinguishing features are shown in the following table:

G command

Wear value

Active orientable tool carrier

TOWSTD:

Initial value, tool length

Wear values are subject to rotation.

TOWMCS:

Wear value in MCS. TOWMCS is iden-

It only rotates the vector of the resul-

tical to TOWSTD if a tool carrier that

tant tool length without taking into

can be orientated is not active.

account the wear.

TOWWCS:

The wear value is converted to the

The tool vector is calculated as for

MCS in the WCS.

TOWMCS without taking into account

the wear.

TOWBCS:

The wear value is converted to the

The tool vector is calculated as for

MCS in the BCS.

TOWMCS without taking into account

the wear.

TOWTCS:

The wear value is converted to the

The tool vector is calculated as for

MCS in the workpiece coordinate sys-

TOWMCS without taking into account

tem.

the wear.

TOWWCS, TOWBCS, TOWTCS: The wear vector is added to the tool vector.

Linear transformation

The tool length can be defined meaningfully in the MCS only if the MCS is generated by linear

transformation from the BCS.

Non-linear transformation

For example, if with TRANSMIT a non-linear transformation is active, then when specifying

the MCS as requested coordinate system, BCS is automatically used.

No kinematic transformation and no orientable tool carrier

If neither a kinematic transformation nor an orientable tool carrier is active, then all the other

four coordinate systems (except for the WCS) are combined. It is then only the WCS, which

is different to the other systems. Since only tool lengths need to be evaluated, translations

between the coordinate systems are irrelevant.

References:

For more information on tool compensation, see:

Function Manual Basic Functions; Tool Offset (W1)

Inclusion of wear values in calculation

The setting data SD42935 $SC_WEAR_TRANSFORM defines which of the three wear

components:

● Wear

● Total offsets fine

● Total offsets coarse

Job Planning

410

Programming Manual, 12/2018, A5E40869460B AB

Tool offsets

11.3 Special handling of tool offsets

19

Z

Y

X

-17

X

Y

Z

-18

Z

X

Y

-19

Y

Z

X

*)

Each value not equal to 0, which is not equal to one of the six listed values, is evaluated as value 18.

The following table shows the assignment of tool length components to geometry axes for all

other tools (tool types < 400 or > 599):

Operating plane

Length 1

Length 2

Length 3

*)

Z

Y

X

18

Y

X

Z

19

X

Z

Y

-17

Z

X

Y

-18

Y

Z

X

-19

X

Y

Z

*)

Each value not equal to 0, which is not equal to one of the six listed values, is evaluated as value 17.

Note

For representation in tables, it is assumed that geometry axes up to 3 are designated with X,

Y, Z. The axis order and not the axis identifier determines the assignment between a

compensation and an axis.

Job Planning

412

Programming Manual, 12/2018, A5E40869460B AB

Tool offsets

11.4 Online tool offset

11.4

Online tool offset

11.4.1

Defining a polynomial function (FCTDEF)

Certain dressing strategies (e.g. dressing roller) are characterized by the fact that the grinding

wheel radius is continuously (linearly) reduced as the dressing roller is fed in. This strategy

requires a linear function between infeed of the dressing roller and writing the wear value of

each length. The linear function is defined using the predefined procedure FCTDEF(...) for up

to third order polynomial functions.

Straight line equation

y = f(x) = a₀ + a₁*x₁

a₁: Gradient of the straight line, with a₁= Δx / Δy

a₀: Shift of the straight line along the X axis with a₀ = -a1 * X_V

<

˂\

˂[

;

;₉

Syntax

FCTDEF(<Func>,<LLimit>,<ULimit>,<a0>,<a1>,<a2>,<a3>)

Meaning

FCTDEF(...):

Defining a polynomial function for PUTFTOCF(...):

y = f(x) = a₀ + a₁*x + a₂*x² + a₃*x³

<Func>:

Function number

Data type:

INT

Range of values:

1, 2, 3

<LLimit>:

Lower limit value

Data type:

REAL

<ULimit>:

Upper limit value

Data type:

REAL

<a0>,<a1>,<a2>,<a3>:

Coefficients of polynomial function

Data type:

REAL

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

413

Tool offsets

11.4 Online tool offset

Example

Definitions

● Function number: 1

● Lower and upper limit value: -100, 100

● Gradient of the characteristic: a₁ = 1

● The operating point should be located at the center of the characteristic. Based on the

setpoint position of axis XA in the WCS at the instant that the function is defined in the NC

program, the characteristic must be shifted in the negative Y direction: a₀ = -a₁ * XA_D = -1

* $AA_IW

● a₂ = a₃ = 0

Characteristic

<

8/

;$_'

;$

//

UL

Upper limit value

LL

Lower limit value

XA_D

Setpoint of axis XA at the time that the function is defined in the NC program

Programming

Program code

Comment

FCTDEF(1,-100,100,-$AA_IW[XA],1)

; Function definition

11.4.2

Write online tool offset continuously (PUTFTOCF)

Using the predefined procedure PUTFTOCF(...), an online tool offset is executed based on a

polynomial function previously defined with FCTDEF(...) (Page 413).

Note

The online tool offset can also be realized using a synchronized action.

For further information, see Function Manual Synchronized Actions.

Job Planning

414

Programming Manual, 12/2018, A5E40869460B AB

Tool offsets

11.4 Online tool offset

Syntax

PUTFTOCF(<Func>,<RefVal>,<ToolPar>,<Chan>,<Sp>)

Meaning

PUTFTOCF(...):

Write online tool offset, continuously block-by-block using the polynomial function

defined with FCTDEF(...)

<Func>:

Function number, defined in the function definition with FCTDEF(...)

Data type:

INT

Range of val-

1, 2, 3

ues:

<RefVal>:

Reference value, from which the offset is to be derived (e.g. setpoint of an axis).

Data type:

VAR REAL

<ToolPar>:

Number of the wear parameter (length 1, 2 or 3) in which the offset value is to be

included.

Data type:

INT

<Chan>:

Number of the channel in which the online tool offset is to take effect.

Note:

Only required if the offset is not to take effect in the active channel.

Data type:

INT

<Sp>:

Number of the spindle for which the online tool offset is to take effect.

Note:

Only required if the offset is to be applied to a non-active grinding wheel rather

than the active tool that is currently in use.

Data type:

INT

11.4.3

Write online tool offset, discrete (PUTFTOC)

Function

Using the predefined procedurePUTFTOC(...), an online tool offset is executed based on a

fixed offset value.

Syntax

PUTFTOC(<CorrVal>,<ToolPar>,<Chan>,<Sp>)

Meaning

PUTFTOC(...):

Write online tool offset

<CorrVal>:

Offset value, which is added to the wear parameter.

Data type:

REAL

<ToolPar>:

Number of the wear parameter (length 1, 2 or 3) in which the offset value is to be

included.

Data type:

INT

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

415

Tool offsets

11.4 Online tool offset

<Chan>:

Number of the channel in which the online tool offset is to take effect.

Note:

Only required if the offset is not to take effect in the active channel.

Data type:

INT

<Sp>:

Number of the spindle for which the online tool offset is to take effect.

Note:

Only required if the offset is to be applied to a non-active grinding wheel rather

than the active tool that is currently in use.

Data type:

INT

11.4.4

Activate/deactivate online tool offset (FTOCON/FTOCOF)

The online tool offset is activated or deactivated using the G commands FTOCON and

FTOCOF.

Syntax

FTOCON

FTOCOF

Meaning

FTOCON:

Activate online tool offset

The command must be programmed in the channel in which the online tool offset

is to be activated.

FTOCOF:

Deactivate online tool offset

The command must be programmed in the channel in which the online tool offset

is to be deactivated.

Note:

On FTOCOF, the axis does not move further out for the tool offset. However, the

value calculated with PUTFTOC/PUTFTOCF remains in the cutting-specific offset

data.

To finally deactivate the online tool offset, the tool (T...) must again be selected/

deselected after FTOCOF.

Job Planning

416

Programming Manual, 12/2018, A5E40869460B AB

Tool offsets

11.5 3D tool radius compensation

11.5

3D tool radius compensation

11.5.1

Selecting 3D tool radius compensation for 3D circumferential milling (CUT3DC,

CUT3DCD, ISD)

The 3D tool radius compensation (3D TRC) for the 3D circumferential milling without taking

limitation surfaces into account is selected with the modally effective G command CUT3DC or

CUT3DCD.

The actual activation is performed with G41 or G42 The tool radius compensation is

deactivated with G40.

Syntax

G41/G42 ORIC/ORID ISD=... CUT3DC/CUT3DCD CDOF2 X... Y... Z...

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

Meaning

CUT3DC:

3D TRC for circumferential milling (only when 5-axis transforma-

tion is active)

CUT3DCD:

3D TRC for circumferential milling referred to a differential tool

(only when 5-axis transformation is active)

The radius difference is specified by the tool parameter

$TC_DP15.

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

ORIC/ORID:

The behavior for orientation changes at outside corners is speci-

fied via the G commands ORIC and ORID.

ORIC:

Orientation changes at outside corners are superim-

posed on the circle block to be inserted.

ORID:

Orientation changes at outside corners are executed

before the circle block to be inserted.

ISD=<Value>:

With the ISD address, the insertion depth of the tool can be

changed for circumferential milling and active 3D tool radius com-

pensation.

<Value>:

Length of the insertion depth

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

Deactivate tool radius compensation

Note:

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

geometry axis movements.

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

417

Tool offsets

11.5 3D tool radius compensation

$

%

=

;

<

Figure 11-1

Circumferential milling

Approach behavior

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

Behavior at outside corners

The G commands of group 18 (corner behavior, tool offset) are evaluated at the outside corners

for circumferential milling with 3D TRC in the same way as for the conditions for the 2½D TRC:

● G450: Transition circle (tool travels round workpiece corners on a circular path)

In contrast to the solution for the 2½D TRC, the inserted contour element at an outside

corner is always a circle with a 0 radius, on which the tool radius compensation acts in the

same way as on any other programmed path. It is not possible to insert conics instead of

circles. In this case, the DISC address has no significance and is therefore not evaluated.

● G451: Intersection of equidistant paths (tool backs off from the workpiece corner)

The intersection is determined by extending the offset curves of the two participating blocks

and defining the intersection of the two blocks at the corner in the plane perpendicular to

the tool orientation.

The intersection procedure (G451) is not used when at least one block containing a change

to the tool orientation was inserted between the relevant traversing blocks. In this case, a circle

is always inserted at the corner.

Behavior for changes in orientation at outside corners

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

programmed between two blocks forming the corner are executed before the inserted circle

block (ORID) is processed or at the same time (ORIC).

Insertion depth

The insertion depth of the milling tool is the distance of the milling tool reference point from

the tip of the tool.

The milling tool reference point is the vertical projection of the milling tool machining point on

the programmed path to the longitudinal axis of the tool.

Job Planning

Programming Manual, 12/2018, A5E40869460B AB

419

Content      ..     4      5      6      7     ..