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

Transformations

6.2 Three, four and five axis transformation (TRAORI)

Parameter

ORIPLANE

Interpolation in the plane (large-radius circular interpolation)

ORICONCW

Interpolation on the peripheral surface of a taper in the

clockwise direction

ORICONCCW

Interpolation on the peripheral surface of a taper in the

counterclockwise 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 smaller 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)

PHI

Angle of rotation of the orientation about the direction axis of

the taper

PSI

Opening angle of the taper

Possible polynomials

Apart from the different angles, polynomials can also be

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

programmed up to the 5th degree

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

Example of different changes to orientation

…

N10 G1 X0 Y0 F5000

N20 TRAORI(1)

; Orientation transformation on.

N30 ORIVECT

; Interpolate tool orientation as a vector.

…

; Tool orientation in the plane.

N40 ORIPLANE

; Select large-radius circular interpolation.

N50 A3=0 B3=0 C3=1

N60 A3=0 B3=1 C3=1

; Orientation in the Y/Z plane is rotated

through 45 degrees, orientation (0,1, 2,1/√2,

1/√2) is reached at the end of the block.

…

N70 ORICONCW

; Orientation programming on the outside of the

taper:

N80 A6=0 B6=0 C6=1 A3=0 B3=0 C3=1

; The orientation vector is interpolated on the

outside of a taper with the direction (0,0,1)

up to the orientation (1/√2,0,1/√2) in the

clockwise sense, the angle of rotation is

270 degrees.

N90 A6=0 B6=0 C6=1

; The tool orientation goes through a full

revolution on the outside of the same taper.

Job Planning

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

337

Transformations

6.2 Three, four and five axis transformation (TRAORI)

Description

If changes of orientation along the peripheral surface of a taper anywhere in space are to be

described, the vector about which the tool orientation is to be rotated must be known. The

start and end orientation must also be specified. The start orientation results from the

previous block and the end orientation has to be programmed or defined via other

conditions.

Programming in the ORIPLANE plane corresponds to ORIVECT

The programming of large-radius circular interpolation together with angle polynomials

corresponds to the linear and polynomial interpolation of contours. The tool orientation is

interpolated in a plane that is defined by the start and end orientation. If additional

polynomials are programmed, the orientation vector can also be tilted out of the plane.

Programming of circles in a plane G2/G3, CIP and CT

The extended orientation corresponds to the interpolation of circles in a plane. For the

corresponding programming options for circles with centers or radii such as G2/G3, circle via

intermediate point CIP and tangential circles CT, see

References: Programming Manual Fundamentals, "Programming motion commands".

Orientation programming

Interpolation of the orientation vector on the peripheral surface of a taper ORICONxx

Four different types of interpolation from G-code group 51 can be selected for interpolating

orientations on the peripheral surface of a taper:

1. Interpolation on the outside of a taper in the clockwise direction ORICONCW with

specification of end orientation and taper direction, or opening angle. The direction vector

is programmed with identifiers A6, B6, C6 and the opening angle of the taper with

identifier NUT= value range in interval 0 degrees to 180 degrees.

2. Interpolation on the outside of a taper in the counterclockwise direction ORICONCCW with

specification of end orientation and taper direction, or opening angle. The direction vector

is programmed with identifiers A6, B6, C6 and the opening angle of the taper with

identifier NUT= value range in interval 0 degrees to 180 degrees.

3. Interpolation on the outside of a taper ORICONIO with specification of end orientation and

an intermediate orientation, which is programmed with identifiers A7, B7, C7.

4. Interpolation on the outside of a taper ORICONTO with tangential transition and specification

of end orientation. The direction vector is programmed with identifiers A6, B6, C6.

Job Planning

338

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

Transformations

6.2 Three, four and five axis transformation (TRAORI)

6.2.9

Specification of orientation for two contact points (ORICURVE, PO[XH]=,

PO[YH]=, PO[ZH]=)

Function

Programming the change in orientation using the second curve in space ORICURVE

Another way to program changes in orientation, besides using the tool tip along a curve in

space, is to program the motion of a second contact point of the tool using ORICURVE. In this

way, changes in tool orientation can be defined uniquely, as when programming the tool

vector itself.

Machine manufacturer

Please refer to the machine manufacturer's notes on axis identifiers that can be set via

machine data for programming the second orientation path of the tool.

Programming

This type of interpolation can be used to program points (using G1) or polynomials (using

POLY) for the two curves in space. Circles and involutes are not permitted. A BSPLINE spline

interpolation and the "Combine short spline blocks" function can also be activated.

References:

/FB1/ Function Manual, Basic Functions; Continuous-Path Mode, Exact Stop, Look Ahead

(B1), chapter: Combine short spline blocks

The other spline types, ASPLINE and CSPLINE, and compressor activation using COMPON,

COMPCURV or COMPCAD are not permitted.

The motion of the two contact points of the tool can be predefined up to the 5th degree when

programming the orientation polynomials for coordinates.

Extended orientation interpolation with additional curve in space and polynomials for

coordinates

N... ORICURVE

Specification of the motion of the second

N... PO[XH]=(xe, x2, x3, x4, x5)

contact point of the tool and additional

N... PO[YH]=(ye, y2, y3, y4, y5)

N... PO[ZH]=(ze, z2, z3, z4, z5)

polynomials of the coordinates in

question

Job Planning

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

339

Transformations

6.2 Three, four and five axis transformation (TRAORI)

Parameters

ORICURVE

Interpolation of the orientation specifying a movement

between two contact points of the tool

XH YH ZH

Identifiers of the coordinates of the second contact

point of the tool of the additional contour as a curve

in space

Possible polynomials

Apart from using the appropriate end points, the curves

PO[XH]=(xe, x2, x3, x4,

in space can also be programmed using polynomials.

x5) PO[YH]=(ye, y2, y3,

y4, y5) PO[ZH]=(ze, z2,

z3, z4, z5)

xe, ye, ze

End points of the curve in space

xi, yi, zi

Coefficients of the polynomials up to the 5th degree

Note

Identifiers XH YH ZH for programming a second orientation path

The identifiers must be selected such that no conflict arises with the other identifiers or linear

axes

X Y Z axes

and rotary axes such as

A2 B2 C2 Euler angle or RPY angle

A3 B3 C3 direction vectors

A4 B4 C4 or A5 B5 C5 surface normal vectors

A6 B6 C6 rotation vectors or A7 B7 C7 intermediate point coordinates

or other interpolation parameters.

Job Planning

340

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

Transformations

6.3 Orientation polynomials (PO[angle], PO[coordinate])

6.3

Orientation polynomials (PO[angle], PO[coordinate])

Function

Irrespective of the polynomial interpolation from G-code group 1 that is currently active, two

different types of orientation polynomial can be programmed up to the 5th degree for a 3-axis

to 5-axis transformation.

1. Polynomials for angles: lead angle LEAD, tilt angle TILT

in relation to the plane that is defined by the start and end orientation.

2. Polynomials for coordinates: XH, YH, ZH of the second curve in space for the tool

orientation of a reference point on the tool.

With a 6-axis transformation, the rotation of rotation vector THT can be programmed with

polynomials up to the 5th degree for rotations of the tool itself, in addition to the tool

orientation.

Syntax

Type 1 orientation polynomials for angles

N… PO[PHI]=(a2, a3, a4, a5)

3-axis to 5-axis transformation

N… PO[PSI]=(b2, b3, b4, b5)

3-axis to 5-axis transformation

Type 2 orientation polynomials for coordinates

N… PO[XH]=(xe, x2, x3, x4, x5)

Identifiers for the coordinates of the second

N… PO[YH]=(ye, y2, y3, y4, y5)

orientation path for tool orientation

N… PO[ZH]=(ze, z2, z3, z4, z5)

In both cases, with 6-axis transformations, a polynomial can also be programmed for the

rotation using

N… PO[THT]=(c2, c3, c4, c5)

Interpolation of the rotation relative to the

path

N… PO[THT]=(d2, d3, d4, d5)

Interpolation absolute, relative and

tangential to the change of orientation

of the orientation vector. This is possible if the transformation supports a rotation vector with

an offset that can be programmed and interpolated using the THETA angle of rotation.

Job Planning

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

341

Transformations

6.3 Orientation polynomials (PO[angle], PO[coordinate])

Meaning

PO[PHI]

Angle in the plane between start and end orientation

PO[PSI]

Angle describing the tilt of the orientation from the plane between start and end

orientation

PO[THT]

Angle of rotation created by rotating the rotation vector of one of the G codes

of group 54 that is programmed using THETA

PHI

Lead angle LEAD

PSI

Tilt angle TILT

THETA

Rotation about the tool direction in Z

PO[XH]

X coordinate of the reference point on the tool

PO[YH]

Y coordinate of the reference point on the tool

PO[ZH]

Z coordinate of the reference point on the tool

Description

Orientation polynomials cannot be programmed:

● If ASPLINE, BSPLINE, CSPLINE spline interpolations are active.

Type 1 polynomials for orientation angles are possible for every type of interpolation

except spline interpolation, that is, linear interpolation with rapid traverse G00 or with

feedrate G01

with polynomial interpolation using POLY and

circular/involute interpolation G02, G03, CIP, CT, INVCW and INCCCW.

However, type 2 polynomials for orientation coordinates are only possible if

linear interpolation with rapid traverse G00 or with feedrate G01 or

polynomial interpolation with POLY is active.

● If the orientation is interpolated using ORIAXES axis interpolation. In this case, polynomials

can be programmed directly with PO[A] and PO[B] for orientation axes A and B.

Type 1 orientation polynomials with ORIVECT, ORIPLANE and ORICONxx

Only type 1 orientation polynomials are possible for large-radius circular interpolation and

interpolation outside of the taper with ORIVECT, ORIPLANE and ORICONxx.

Type 2 orientation polynomials with ORICURVE

If interpolation with the additional curve in space ORICURVE is active, the Cartesian

components of the orientation vector are interpolated and only type 2 orientation polynomials

are possible.

Job Planning

342

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

Transformations

6.4 Rotations of the tool orientation (ORIROTA, ORIROTR, ORIROTT, ORIROTC, THETA)

6.4

Rotations of the tool orientation (ORIROTA, ORIROTR, ORIROTT,

ORIROTC, THETA)

Function

If you also want to be able to change the orientation of the tools on machine types with

movable tools, program each block with end orientation. Depending on the machine

kinematics you can either program the orientation direction of the orientation axes or the

direction of rotation of orientation vector THETA. Different interpolation types can be

programmed for these rotation vectors:

● ORIROTA: Angle of rotation to an absolute direction of rotation.

● ORIROTR: Angle of rotation relative to the plane between the start and end orientation.

● ORIROTT: Angle of rotation relative to the change in the orientation vector.

● ORIROTC: Tangential angle of rotation to the path tangent.

Syntax

Only if interpolation type ORIROTA is active can the angle of rotation or rotation vector be

programmed in all four modes as follows:

1. Directly as rotary axis positions A, B, C

2. Euler angles (in degrees) with A2, B2, C2

3. RPY angles (in degrees) with A2, B2, C2

4. Direction vector via A3, B3, C3 (angle of rotation using THETA=value)

If ORIROTR or ORIROTT is active, the angle of rotation can only be programmed directly with

THETA.

A rotation can also be programmed in a separate block without an orientation change taking

place. In this case, ORIROTR and ORIROTT are irrelevant. In this case, the angle of rotation is

always interpreted with reference to the absolute direction (ORIROTA).

N... ORIROTA

Define the interpolation of the rotation vector

N... ORIROTR

N... ORIROTT

N... ORIROTC

N... A3= B3= C3= THETA=value

Define the rotation of the orientation vector

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

Interpolate angle of rotation with a 5th order

polynomial

Job Planning

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

343

Transformations

6.4 Rotations of the tool orientation (ORIROTA, ORIROTR, ORIROTT, ORIROTC, THETA)

Significance

ORIROTA

Angle of rotation to an absolute direction of rotation.

ORIROTR

Angle of rotation relative to the plane between the start and end

orientation.

ORIROTT

Angle of rotation as a tangential rotation vector to the change of orientation

ORIROTC

Angle of rotation as a tangential rotation vector to the path tangent

THETA

Rotation of the orientation vector

THETA=value

Angle of rotation in degrees reached by the end of the block

THETA=Θe

Angle of rotation with end angle Θe of rotation vector

THETA=AC(...)

Non-modal switchover to absolute dimensions

THETA=AC(…)

Non-modal switchover to incremental dimensions

Θe

End angle of rotational vector both absolute with G90 and relative with

G91 (incremental dimensioning) is active

PO[THT]=(

) Polynomial for angle of rotation

Example of rotations of orientations

Program code

Comments

N10 TRAORI

; Activate orientation transformation

N20 G1 X0 Y0 Z0 F5000

; Tool orientation

N30 A3=0 B3=0 C3=1 THETA=0

; In Z direction with angle of rotation 0

N40 A3=1 B3=0 C3=0 THETA=90

; In X direction and rotation about 90 degrees

N50 A3=0 B3=1 C3=0 PO[THT]=(180,90)

; Orientation

N60 A3=0 B3=1 C3=0 THETA=IC(-90)

; In Y direction and rotation about 180

degrees

N70 ORIROTT

; Remains constant and rotation to 90 degrees

N80 A3=1 B3=0 C3=0 THETA=30

; Angle of rotation relative to change of

orientation

; Rotation vector in angle 30 degrees to X/Y

plane

When interpolating block

N40, the angle of rotation from initial value of 0 degrees to final value of 90 degrees is

interpolated linearly. In block N50, the angle of rotation changes from 90 degrees to 180

degrees, according to

parabola θ(u) = +90u². In N60, a rotation can also be executed without a change in

orientation taking place.

With N80, the tool orientation is rotated from the Y direction toward the X direction. The

change in orientation takes place in the X/Y plane and the rotation vector describes an angle

of 30 degrees to this plane.

Job Planning

344

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

Transformations

6.4 Rotations of the tool orientation (ORIROTA, ORIROTR, ORIROTT, ORIROTC, THETA)

Description

ORIROTA

The angle of rotation THETA is interpolated with reference to an absolute direction in space.

The basic direction of rotation is defined in the machine data.

ORIROTR

The angle of rotation THETA is interpreted relative to the plane defined by the start and end

orientation.

ORIROTT

The angle of rotation THETA is interpreted relative to the change in orientation. For THETA=0

the rotation vector is interpolated tangentially to the change in orientation and only differs

from ORIROTR if at least one polynomial has been programmed for "tilt angle PSI" for the

orientation. The result is a change in orientation that is not executed in the plane. An

additional angle of rotation THETA can then be used to interpolate the rotation vector such that

it always produces a specific value referred to the change in orientation.

ORIROTC

The rotation vector is interpolated relative to the path tangent with an offset that can be

programmed using the THETA angle. A polynomial PO[THT]=(c2, c3, c4, c5) up to the 5th

degree can also be programmed for the offset angle.

Job Planning

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

345

Transformations

6.5 Orientations relative to the path

6.5

Orientations relative to the path

6.5.1

Orientation types relative to the path

Function

By using this expanded function, relative orientation is not only achieved at the end of the

block, but across the entire trajectory. The orientation achieved in the previous block is

transferred to the programmed end orientation using large-radius circular interpolation. There

are basically two ways of programming the desired orientation relative to the path:

1. Like the tool rotation, the tool orientation is interpolated relative to the path using

ORIPATH, ORPATHTS.

2. The orientation vector is programmed and interpolated in the usual manner. The rotation

of the orientation vector is initiated relative to the path tangent using ORIROTC.

Syntax

The type of interpolation of the orientation and the rotation of the tool is programmed using:

N... ORIPATH

Orientation relative to the path

N... ORIPATHS

Orientation relative to the path with smoothing of

orientation characteristic

N... ORIROTC

Interpolation of the rotation vector relative to the

path

An orientation blip caused by a corner on the trajectory can be smoothed using ORIPATHS.

The direction and path length of the retracting movement is programmed via the vector using

the components A8=X, B8=Y C8=Z.

Job Planning

346

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

Transformations

6.5 Orientations relative to the path

ORIPATH/ORIPATHS can be used to program various references to the path tangent via the

three angles

● LEAD= Specification of lead angle relative to the path and surface

● TILT= Specification of tilt angle relative to the path and surface

● THETA= Angle of rotation

for the entire trajectory. Polynomials up to the 5th degree can be programmed in addition to

the THETA angle of rotation using PO[THT]=(...).

Note

Machine manufacturer

Please refer to the machine manufacturer's instructions. Other settings can be made for

orientations relative to the path via configurable machine and setting data. For more detailed

information, please refer to

References:

/FB3/ Function Manual, Special Functions; 3 to 5-Axis Transformation (F2),

Chapter "Orientation"

Significance

Various settings can be made for the interpolation of angles LEAD and TILT via machine data:

● The tool-orientation reference programmed using LEAD and TILT is retained for the entire

block.

● Lead angle LEAD: rotation about the direction vertical to the tangent and normal vector

TILT: rotation of the orientation about the normal vector.

● Lead angle LEAD: rotation about the direction vertical to the tangent and normal vector Tilt

angle TILT: rotation of the orientation in the direction of the path tangent.

● Angle of rotation THETA: rotation of the tool about itself with an additional third rotary axis

acting as an orientation axis in 6-axis transformation.

Note

Orientation relative to the path not permitted in conjunction with OSC, OSS, OSSE, OSD

and OST

Orientation interpolation relative to the path, that is ORIPATH or ORIPATHS and ORIOTC,

cannot be programmed in conjunction with orientation characteristic smoothing with a G

code from group 34. OSOF has to be active for this.

Job Planning

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

347

Transformations

6.5 Orientations relative to the path

6.5.2

Rotation of the tool orientation relative to the path (ORIPATH, ORIPATHS,

angle of rotation)

Function

With a 6-axis transformation, the tool can be rotated about itself with a third rotary axis to

orientate the tool as desired in space. With a rotation of the tool orientation relative to the

path using ORIPATH or ORIPATHS, the additional rotation can be programmed via the

THETA angle of rotation. Alternatively, the LEAD and TILT angles can be programmed using

a vector, which is located in the plane vertical to the tool direction.

Machine manufacturer

Please refer to the machine manufacturer's instructions. The interpolation of the LEAD and

TILT angles can be set differently using machine data.

Syntax

Rotation of tool orientation and tool

The type of tool orientation relative to the path is activated using ORIPATH or ORIPATHS.

N... ORIPATH

Activate type of orientation relative to the path

N... ORIPATHS

Activate type of orientation relative to the path

with smoothing of the orientation characteristic

Activating the three angles that can be rotated:

N... LEAD=

Angle for the programmed orientation relative to

the surface normal vector

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

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

Polynomial for the tilt angle TILT

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

Polynomial for the angle of rotation

THETA

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

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

Job Planning

348

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

Transformations

6.5 Orientations relative to the path

Significance

Tool orientation relative to the path

ORIPATH Tool orientation in relation to path

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

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.

6.5.3

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

Function

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 rotation. A polynomial can, therefore, be programmed up to the 5th degree for the

offset angle using PO[THT].

Syntax

N... ORIROTC

Initiate the rotation of the tool relative

to the path tangent

N... A3= B3= C3= THETA=value

Define the rotation of the orientation

vector

N... A3= B3= C3= PO[THT]=(c2, c3, c4, c5)

Interpolate offset angle with

polynomial up to 5th degree

A rotation can also be programmed in a separate block without an orientation change taking

place.

Job Planning

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

349

Transformations

6.5 Orientations relative to the path

Significance

Interpolation of the rotation of tool relative to the path in 6-axis transformation

ORIROTC

Initiate tangential rotation vector relative to path tangent

THETA=value

Angle of rotation in degrees reached by the end of the block

THETA=θe

Angle of rotation with end angle Θe of rotation vector

THETA=AC(…)

Switch over to absolute dimensions per block

THETA=IC(…)

Switch over to incremental dimensions per block

PO[THT]=(c2, c3, c4, c5) Interpolate offset angle with polynomial of 5th degree

Note

Interpolation of the rotation vector ORIROTC

Initiating rotation of the tool relative to the path tangent in the opposite direction to the tool

orientation, is only possible with a 6-axis transformation.

With active ORIROTC

Rotation vector ORIROTA cannot be programmed. If programming is undertaken, ALARM

14128 "Absolute programming of tool rotation with active ORIROTC" is output.

Orientation direction of the tool for 3-axis to 5-axis transformation

The orientation direction of the tool can be programmed via Euler angles, RPY angles or

direction vectors as with 3-axis to 5-axis transformations. Orientation changes of the tool in

space can also be achieved by programming the large-radius circular interpolation

ORIVECT, linear interpolation of the orientation axes ORIAXES, all interpolations on the

peripheral surface of a taper ORICONxx, and interpolation in addition to the curve in space

with two contact points of the tool ORICURVE.

Details of the rotary axis motion

X Y Z

Details of the linear axes

ORIAXES

Linear interpolation of machine or orientation axes

ORIVECT

Large-radius circular 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

Job Planning

350

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

Transformations

6.5 Orientations relative to the path

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-radius circular interpolation)

ORICONCW

Interpolation on the peripheral surface of a taper in the

clockwise direction

ORICONCCW

Interpolation on the peripheral surface of a taper in the

counterclockwise 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 smaller 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

XH YH ZH, e.g., with

two contact points of the tool. In addition to the end points,

polynomials

additional curve polynomials can also be programmed.

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.

6.5.4

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

Function

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, 03/2010, 6FC5398-2BP20-1BA0

351

Transformations

6.5 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 more detailed information about the "Orientation relative to the path" function, please

refer to

References: /FB3/ Function Manual, Special Functions; 3- to 5-Axis Transformation (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

Significance

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-radius circular interpolation.

Job Planning

352

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

Transformations

6.6 Compression of the orientation (COMPON, COMPCURV, COMPCAD)

6.6

Compression of the orientation (COMPON, COMPCURV,

COMPCAD)

Function

NC programs, in which orientation transformation (TRAORI) is active, and the orientation is

programmed using direction vectors, can be compressed if kept within specified limits.

Note

The orientation movement is only compressed if large-radius circular interpolation is active

and depends, therefore, on the G code for orientation interpolation. This can be set via

machine data, as can the maximum path length and a permissible tolerance for each axis or

for the path feedrate for the compressor function. Please refer to the machine manufacturer's

instructions.

Programming

Tool orientation

If orientation transformation (TRAORI) is active, for 5-axis machines, tool orientation can be

programmed in the following way (independent of the kinematics):

● Programming of the direction vectors via:

A3=<...> B3=<...> C3=<...>

● Programming of the Euler angles or RPY angles via:

A2=<...> B2=<...> C2=<...>

Rotation of the tool

For six-axis machines you can program the tool rotation in addition to the tool orientation.

The angle of rotation is programmed with:

THETA=<...>

See "Rotation of tool orientation (Page 343)".

Note

NC blocks in which additional rotation is programmed, can only be compressed if the angle

of rotation changes linearly, meaning that a polynomial with PO[THT]=(...) for the angle of

rotation should not be programmed.

Job Planning

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

353

Transformations

6.6 Compression of the orientation (COMPON, COMPCURV, COMPCAD)

General structure of an NC block that be compressed

The general structure of an NC block that can be compressed can therefore look like this:

N... X=<...> Y=<...> Z=<...> A3=<...> B3=<...> C3=<...> THETA=<...> F=<...>

N... X=<...> Y=<...> Z=<...> A2=<...> B2=<...> C2=<...> THETA=<...> F=<...>

Note

The position values can be entered directly (e.g. X90) or indirectly via parameter settings

(e.g. X=R1*(R2+R3)).

Programming tool orientation using rotary axis positions

Tool orientation can be also specified using rotary axis positions, e.g. with the following

structure:

N... X=<...> Y=<...> Z=<...> A=<...> B=<...> C=<...> THETA=<...> F=<...>

In this case, compression is executed in two different ways, dependent on whether large

radius circular interpolation is executed. If no large radius circular interpolation takes place,

then the compressed change in orientation is represented in the usual way by axial

polynomials for the rotary axes.

Contour accuracy

Depending on the selected compression mode (MD20482 $MC_COMPRESSOR_MODE)

either the configured axis-specific tolerances (MD33100 $MA_COMPRESS_POS_TOL) or

the following channel-specific tolerances - set using setting data - are effective for the

geometry axes and orientation axes for compression:

SD42475 $SC_COMPRESS_CONTUR_TOL (maximum contour deviation)

SD42476 $SC_COMPRESS_ORI_TOL (maximum angular deviation for tool orientation)

SD42477 $SC_COMPRESS_ORI_ROT_TOL (maximum angular deviation for the angle of

rotation of the tool) (only available on 6-axis machines)

References:

Function Manual Basic Functions; 3 to 5-Axis Transformation (F2),

Chapter: "Compression of the orientation"

Job Planning

354

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

Transformations

6.6 Compression of the orientation (COMPON, COMPCURV, COMPCAD)

Activation/deactivation

Compressor functions are activated using the modal G codes COMPON, COMPCURV or COMPCAD.

COMPOF terminates the compressor function.

See "NC block compression (COMPON, COMPCURV, COMPCAD) (Page 247)".

Note

Orientation motion is only compressed when large radius circular interpolation is active (i.e.

tool orientation is changed in the plane which is determined by start and end orientation).

Large radius circular interpolation is executed under the following conditions:

• MD21104 $MC_ORI_IPO_WITH_G_CODE = 0,

ORIWKS is active and

the orientation is programmed as a vector (with A3, B3, C3 or A2, B2, C2).

• MD21104 $MC_ORI_IPO_WITH_G_CODE = 1 and

ORIVECT or ORIPLANE is active.

The tool orientation can be programmed either as a direction vector or with rotary axis

positions. If one of the G-codes ORICONxx or ORICURVE is active, or if polynomials for the

orientation angles (PO[PHI] and PO[PSI]) are programmed, no large circle interpolation will

be executed.

Example

In the example program below, a circle approached by a polygon definition is compressed.

The tool orientation moves on the outside of the taper at the same time. Although the

programmed orientation changes are executed one after the other, but in an unsteady way,

the compressor function generates a smooth motion of the orientation.

Job Planning

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

355

Transformations

6.6 Compression of the orientation (COMPON, COMPCURV, COMPCAD)

Programming

Comments

DEF INT NUMBER=60

DEF REAL RADIUS=20

DEF INT COUNTER

DEF REAL ANGLE

N10 G1 X0 Y0 F5000 G64

$SC_COMPRESS_CONTUR_TOL=0.05

; Maximum deviation of the contour = 0.05 mm

$SC_COMPRESS_ORI_TOL=5

; Maximum deviation of the orientation

= 5 degrees

TRAORI

COMPCURV

; The movement describes a circle generated

from polygons. The orientation moves on a

taper around the Z axis with an opening

angle of 45 degrees.

N100 X0 Y0 A3=0 B3=-1 C3=1

N110 FOR COUNTER=0 TO NUMBER

N120 ANGLE=360*COUNTER/NUMBER

N130 X=RADIUS*cos(angle) Y=RADIUS*sin(angle)

A3=sin(angle) B3=-cos(angle) C3=1

N140 ENDFOR

Job Planning

356

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

Transformations

6.7 Smoothing the orientation characteristic (ORISON, ORISOF)

6.7

Smoothing the orientation characteristic (ORISON, ORISOF)

Function

The "Smoothing the orientation characteristic (ORISON)" function can be used to smooth

oscillations affecting orientation over several blocks. The aim is to achieve a smooth

characteristic for both the orientation and the contour.

Condition

The "Smoothing the orientation characteristic (ORISON)" function is only available in

systems with 5-/6-axis transformation.

Syntax

ORISON

ORISOF

Significance

ORISON:

Smoothing of the orientation characteristic ON

Effective:

modal

ORISOF:

Smoothing of the orientation characteristic OFF

Effective:

modal

Setting data

The orientation characteristic is smoothed conforming to:

● A predefined maximum tolerance (maximum angular deviation of the tool orientation in

degrees)

and

● A predefined maximum path distance

These specifications are defined in setting data:

● SD42678 $SC_ORISON_TOL (tolerance for smoothing the orientation characteristic)

● SD42680 O$SC_ORISON_DIST (path distance for smoothing the orientation

characteristic)

Job Planning

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

357

Transformations

6.7 Smoothing the orientation characteristic (ORISON, ORISOF)

Example

Program code

Comments

TRAORI()

; Activation of orientation transformation.

ORISON

; Activation of orientation smoothing.

$SC_ORISON_TOL=1.0

; Orientation tolerance smoothing = 1.0 degrees.

G91

X10 A3=1 B3=0 C3=1

X10 A3=-1 B3=0 C3=1

X10 A3=1 B3=0 C3=1

X10 A3=-1 B3=0 C3=1

X10 A3=1 B3=0 C3=1

X10 A3=-1 B3=0 C3=1

X10 A3=1 B3=0 C3=1

X10 A3=-1 B3=0 C3=1

X10 A3=1 B3=0 C3=1

X10 A3=-1 B3=0 C3=1

ORISOF

; Deactivation of orientation smoothing.

The orientation is pivoted through 90 degrees on the XZ plane from -45 to +45 degrees. Due

to the smoothing of the orientation characteristic the orientation is no longer able to reach the

maximum angle values of -45 or +45 degrees.

Further information

Number of blocks

The orientation characteristic is smoothed over a configured number of blocks set in

machine data MD28590 $MC_MM_ORISON_BLOCKS.

Note

If smoothing of the orientation characteristic is activated with ORISON without sufficient block

memory having been configured for it (MD28590 < 4), an alarm signal will be output and the

function cannot be executed.

Maximum block path length

The orientation characteristic is only smoothed in blocks whose traversing distance is shorter

than the configured maximum block path length

(MD20178 $MC_ORISON_BLOCK_PATH_LIMIT). Blocks with longer traversing distances

interrupt smoothing and are traversed as programmed.

Job Planning

358

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

Transformations

6.8 Kinematic transformation

6.8

Kinematic transformation

6.8.1

Milling on turned parts (TRANSMIT)

Function

The TRANSMIT function enables the following:

● Face machining on turned parts in the turning clamp (drill-holes, contours).

● A cartesian coordinate system can be used to program these machining operations.

● The control maps the programmed traversing movements of the Cartesian coordinate

system onto the traversing movements of the real machine axes (standard situation):

- Rotary axis

- Infeed axis perpendicular to rotary axis

- Longitudinal axis parallel to rotary axis

- The linear axes are positioned perpendicular to one another.

● A tool center offset relative to the turning center is permitted.

● The velocity control makes allowance for the limits defined for the rotations.

Job Planning

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

359

Transformations

6.8 Kinematic transformation

TRANSMIT transformation types

The TRANSMIT machining operations have two parameterizable forms:

● TRANSMIT in the standard case with (TRAFO_TYPE_n = 256)

● TRANSMIT with additional Y linear axis (TRAFO_TYPE_n = 257)

The extended transformation type 257 can be used, for example, to compensate clamping

compensations of a tool with real Y axis.

Syntax

TRANSMIT or TRANSMIT(n)

TRAFOOF

Rotary axis

The rotary axis cannot be programmed because it is occupied by a geometry axis and

cannot thus be programmed directly as a channel axis.

Significance

TRANSMIT:

Activates the first declared TRANSMIT function. This function is also

designated as polar transformation.

TRANSMIT(n):

Activates the nth declared TRANSMIT function; n can be up to 2

(TRANSMIT(1) is the same as TRANSMIT).

TRAFOOF:

Deactivates an active transformation.

OFFN:

Offset contour normal: Distance of the face machining from the

programmed reference contour.

Note

An active TRANSMIT transformation is likewise deactivated if one of the other transformations

is activated in the relevant channel (e.g., TRACYL, TRAANG, TRAORI).

Job Planning

360

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

Transformations

6.8 Kinematic transformation

Example

;

Program code

Comments

N10 T1 D1 G54 G17 G90 F5000 G94

; Tool selection

N20 G0 X20 Z10 SPOS=45

; Approach the starting position

N30 TRANSMIT

; Activate TRANSMIT function

N40 ROT RPL=-45

; Set frame

N50 ATRANS X-2 Y10

N60 G1 X10 Y-10 G41 OFFN=1OFFN

; Square roughing; 1 mm tolerance

N70 X-10

N80 Y10

N90 X10

N100 Y-10

N110 G0 Z20 G40 OFFN=0

; Tool change

N120 T2 D1 X15 Y-15

N130 Z10 G41

N140 G1 X10 Y-10

; Square finishing

N150 X-10

N160 Y10

N170 X10

N180 Y-10

N190 Z20 G40

; Deselect frame

N200 TRANS

N210 TRAFOOF

N220 G0 X20 Z10 SPOS=45

; Approach the starting position

N230 M30

Job Planning

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

361

Transformations

6.8 Kinematic transformation

Description

Pole

There are two ways of passing through the pole:

● Traversal along linear axis

● Traverse to the pole, rotate the rotary axis at the pole and traveling away from the pole

Make the selection using MD 24911 and 24951.

TRANSMIT with additional Y linear axis (transformation type 257):

This transformation variant of the polar transformation makes use of the redundancy for a

machine with another linear axis in order to perform an improved tool compensation. The

following conditions then apply to the second linear axis:

● A smaller working area and

● The second linear axis should not be used for the retraction of the parts program.

Certain machine data settings are assumed for the parts program and the assignment of the

corresponding axes in the BCS or MCS, see

References

/FB2/ Function Manual Extended Functions; Kinematic Transformations (M1)

6.8.2

Cylinder surface transformation (TRACYL)

Function

The TRACYL cylinder surface transformation function can be used to:

Machine

● longitudinal grooves on cylindrical bodies,

● Transverse grooves on cylindrical objects,

● grooves with any path on cylindrical bodies.

The path of the grooves is programmed with reference to the unwrapped, level surface of the

cylinder.

Job Planning

362

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

Transformations

6.8 Kinematic transformation

;

TRACYL transformation types

There are three forms of cylinder surface coordinate transformation:

● TRACYL without groove wall offset (TRAFO_TYPE_n=512)

● TRACYL with groove wall offset: (TRAFO_TYPE_n=513)

● TRACYL with additional linear axis and groove wall offset: (TRAFO_TYPE_n=514)

The groove wall offset is parameterized with TRACYL using the third parameter.

For cylinder peripheral curve transformation with groove side compensation, the axis used

for compensation should be positioned at zero (y=0), so that the groove centric to the

programmed groove center line is finished.

Axis utilization

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).

Syntax

TRACYL(d) or TRACYL(d, n) or

for transformation type 514

TRACYL(d, n, groove side offset)

TRAFOOF

Rotary axis

The rotary axis cannot be programmed as it is occupied by a geometry axis and thus cannot

be programmed directly as channel axis.

Job Planning

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

363

Transformations

6.8 Kinematic transformation

Significance

TRACYL(d)

Activates the first TRACYL function specified in the channel

machine data. d is the parameter for the working diameter.

TRACYL (d, n)

Activates the n-th TRACYL function specified in the channel

machine data. The maximum for n is 2, TRACYL(d,1)

corresponds to TRACYL(d).

Value for the working diameter. The working diameter is

double the distance between the tool tip and the turning

center. This diameter must always be specified and be larger

than 1.

Optional 2nd parameter for the TRACYL data block 1

(preselected) or 2.

Slot side compensation Optional 3rd parameter whose value for TRACYL is

preselected using the mode for machine data.

Value range:

0: Transformation type 514 without groove wall offset as

1: Transformation type 514 with groove wall offset

TRAFOOF

Transformation OFF (BCS and MCS are once again identical).

OFFN

Offset contour normal: Distance of the groove side from the

programmed reference contour.

Note

An active TRACYL transformation is likewise deactivated if one of the other transformations is

activated in the relevant channel (e.g., TRANSMIT, TRAANG, TRAORI).

Example: Tool definition

The following example is suitable for testing the parameterization of the TRACYL cylinder

transformation:

Program code

Comments

Tool parameters

Significance

Comment

Number (DP)

$TC_DP1[1,1]=120

Tool type

Milling tool

$TC_DP2[1,1]=0

Tool nose position

only for turning tools

Program code

Comments

Geometry

Length compensation

$TC_DP3[1,1]=8.

Length offset vector

Calculation acc. to type

$TC_DP4[1,1]=9.

and plane

$TC_DP5[1,1]=7.

Job Planning

364

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

Transformations

6.8 Kinematic transformation

Program code

Comments

Geometry

Radius

$TC_DP6[1,1]=6.

Radius

Tool radius

$TC_DP7[1,1]=0

Slot width b for slotting

saw, rounding radius for

milling tools

$TC_DP8[1,1]=0

Projection k

For slotting saw only

$TC_DP9[1,1]=0

$TC_DP10[1,1]=0

$TC_DP11[1,1]=0

Angle for taper milling

tools

Program code

Comments

Wear

Tool length and radius

compensation

$TC_DP12[1,1]=0

Remaining parameters to

Tool base dimension/adapter

$TC_DP24=0

Example: Making a hook-shaped groove

;

Job Planning

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

365

Transformations

6.8 Kinematic transformation

Activate cylinder surface transformation:

Program code

Comments

N10 T1 D1 G54 G90 F5000 G94

; Tool selection, clamping compensation

N20 SPOS=0

; Approach the starting position

N30 G0 X25 Y0 Z105 CC=200

N40 TRACYL (40)

; Activate cylinder surface ;transformation

N50 G19

; Plane selection

Machining a hook-shaped groove:

Program code

Comments

N60 G1 X20

; Infeed tool to groove base

N70 OFFN=12

; Define 12 mm groove side spacing relative to

groove center line

N80 G1 Z100 G42

; Approach right side of groove

N90 G1 Z50

; Groove cut parallel to cylinder axis

N100 G1 Y10

; Groove cut parallel to circumference

N110 OFFN=4 G42

; Approach left side of the groove; define 4 mm

groove side spacing relative to the groove

center line

N120 G1 Y70

; Groove cut parallel to circumference

N130 G1 Z100

; Groove cut parallel to cylinder axis

N140 G1 Z105 G40

; Retract from groove wall

N150 G1 X25

; Retract

N160 TRAFOOF

N170 G0 X25 Y0 Z105 CC=200

; Approach the starting position

N180 M30

Job Planning

366

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

Transformations

6.8 Kinematic transformation

Description

Without groove wall offset (transformation type 512):

The control transforms the programmed traversing movements of the cylinder coordinate

system to the traversing movements of the real machine axes:

● Rotary axis

● Infeed axis perpendicular to rotary axis

● Longitudinal axis parallel to rotary axis

The linear axes are positioned perpendicular to one another. The infeed axis cuts the rotary

axis.

RU &0

$60

= RU =0

With groove wall offset (transformation type 513):

Kinematics as above, but an additional longitudinal axis parallel to the peripheral direction

The linear axes are positioned perpendicular to one another.

The velocity control makes allowance for the limits defined for the rotations.

Job Planning

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

367

Transformations

6.8 Kinematic transformation

RU &0

= RU =0

$60

Groove traversing-section

In the case of axis configuration 1, longitudinal grooves along the rotary axis are subject to

parallel limits only if the groove width corresponds exactly to the tool radius.

Grooves in parallel to the periphery (transverse grooves) are not parallel at the beginning

and end.

/RQJLWXGLQDO VORW 7UDQVYHUVH JURRYH

SDUDOOHO OLPLWHG ORQJLWXGL

QDO VORW ZLWK VORW ZDOO

ZLWKRXW JURRYH ZDOO RIIVHW FRPSHQVDWLRQ

75$)2B7<3(BQ

Job Planning

368

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

Transformations

6.8 Kinematic transformation

With additional linear axis and groove wall offset (transformation type 514):

On a machine with a second linear axis, this transformation variant makes use of

redundancy in order to perform improved tool compensation. The following conditions then

apply to the second linear axis:

● a smaller working area and

● the second linear axis should not be used for the travel through the parts program.

Certain machine data settings are assumed for the parts program and the assignment of the

corresponding axes in the BCS or MCS, see

References

/FB2/ Function Manual Extended Functions; Kinematic Transformations (M1)

Offset contour normal OFFN (transformation type 513)

To mill grooves with TRACYL, the following is programmed:

● groove center line in the part program,

● half the groove width programmed using OFFN.

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

active. Furthermore, OFFN should also be >= the tool radius to avoid damage occurring to

the opposite side of the groove.

SURJUDPPHG

2))1

FRQWRXU

Job Planning

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

369

Transformations

6.8 Kinematic transformation

A parts program for milling a groove generally comprises the following steps:

1. Selecting a tool

2. Select TRACYL

3. Select suitable coordinate offset (frame)

4. Position

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.Position

12.TRAFOOF

13.Re-select original coordinate shift (frame)

Special features

● TRC selection:

TRC is not programmed in relation to the groove side, but relative to the programmed

groove center line. To prevent the tool traveling to the left of the groove side, G42 is

entered (instead of G41). You avoid this if in OFFN, the groove width is entered with a

negative sign.

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

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

● It is possible to change OFFN within a parts program. This could be used to shift the

groove center line from the center (see diagram).

● Guiding grooves:

TRACYL does not create the same groove for guiding grooves as it would be with a tool

with the diameter producing the width of the groove. It is basically not possible to create

the same groove side geometry with a smaller cylindrical tool as it is with a larger one.

TRACYL minimizes the error. To avoid problems of accuracy, the tool radius should only be

slightly smaller than half the groove width.

Note

OFFN and TRC

With TRAFO_TYPE_n = 512, the value is effective under OFFN as an allowance for TRC.

With TRAFO_TYPE_n = 513, half the groove width is programmed in OFFN. The contour is

retracted with OFFN-TRC.

Job Planning

370

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

Transformations

6.8 Kinematic transformation

6.8.3

Inclined axis (TRAANG)

Function

The inclined axis function is intended for grinding technology and facilitates the following

performance:

● Machining with an oblique infeed axis

● A Cartesian coordinate system can be used for programming purposes.

● The control maps the programmed traversing movements of the Cartesian coordinate

system onto the traversing movements of the real machine axes (standard situation):

Inclined infeed axis.

༾

;

*ULQGLQJ GLVF

:RUNSLHFH

Syntax

TRAANG(α) or TRAANG(α, n)

TRAFOOF

Significance

TRAANG( ) or

Activate transformation with the parameterization of the previous

TRAANG( ,n)

selection.

TRAANG(α)

Activates the first specified inclined axis transformation

TRAANG(α,n)

Activates the nth agreed inclined axis transformation. The maximum

value of n is 2. TRAANG(α,1) corresponds to TRAANG(α).

Job Planning

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

371

Transformations

6.8 Kinematic transformation

αA

Angle of the inclined axis

Permissible values for α are:

-90 degrees < α < + 90 degrees

TRAFOOF

Transformation off

Number of agreed transformations

Angle α omitted or zero

If α (angle) is omitted (e.g., TRAANG(), TRAANG(, n) ), the transformation is activated with the

parameterization of the previous selection. On the first selection, the default settings

according to the machine data apply.

An angle α = 0 (e.g., TRAANG(0), TRAANG(0,n)) is a valid parameter setting and is no longer

equivalent to the omission of the parameter, as in the case of older versions.

Example

༾

;

*ULQGLQJ GLVF

:RUNSLHFH

Program code

Comments

N10 G0 G90 Z0 MU=10 G54 F5000 ->

; Tool selection, clamping compensation,

-> G18 G64 T1 D1

Plane selection

N20 TRAANG(45)

; Activate inclined axis transformation

N30 G0 Z10 X5

; Approach the starting position

N40 WAITP(Z)

; Release axis for oscillation

N50 OSP[Z]=10 OSP2[Z]=5 OST1[Z]=-2 ->

; Oscillation until the dimension is reached

-> OST2[Z]=-2 FA[Z]=5000

(Oscillation, see Chapter "Oscillation")

N60 OS[Z]=1

N70 POS[X]=4.5 FA[X]=50

N80 OS[Z]=0

Job Planning

372

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

Transformations

6.8 Kinematic transformation

Program code

Comments

N90 WAITP(Z)

; Release oscillating axes as positioning

axes

N100 TRAFOOF

; Deactivate transformation

N110 G0 Z10 MU=10

; Retract

N120 M30

;

-> program in a single block

Description

The following machining operations are possible:

1. Longitudinal grinding

2. Face grinding

3. Grinding of a specific contour

4. Oblique plunge-cut grinding.

Machine manufacturer

The following settings are defined in machine data:

● The angle between a machine axis and the oblique axis,

● The position of the zero point of the tool relative to the origin of the coordinate system

specified by the "inclined axis" function,

● The speed reserve held ready on the parallel axis for the compensating movement,

● The axis acceleration reserve held ready on the parallel axis for the compensating

movement.

Job Planning

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

373

Transformations

6.8 Kinematic transformation

Axis configuration

To program in the Cartesian coordinate system, it is necessary to inform the control of the

correlation between this coordinate system and the actually existing machine axes (MU,MZ):

● Assignment of names to geometry axes

● Assignment of geometry axes to channel axes

- general situation (inclined axis not active)

- inclined axis active

● Assignment of channel axes to machine axis numbers

● Identification of spindles

● Allocation of machine axis names.

Apart from "inclined axis active", the procedure corresponds to the procedure for normal axis

configuration.

6.8.4

Inclined axis programming (G05, G07)

Function

In Jog mode, the movement of the grinding wheel can either be cartesian or in the direction

of the inclined axis (the display stays cartesian). All that moves is the real U axis, the Z axis

display is updated.

In jog-mode, REPOS-offsets must be traversed using Cartesian coordinates.

In jog-mode with active

"PTP-travel", the Cartesian operating range limit is monitored for overtravel and the relevant

axis is braked beforehand. If "PTP travel" is not active, the axis can be traversed right up to

the operating range limit.

References

/FB2/ Description of Functions Extended Functions; Kinematic Transformation (M1)

Syntax

G07

G05

The commands G07/G05 are used to make it easier to program the inclined axes. Positions

can be programmed and displayed in the Cartesian coordinate system. Tool compensation

and zero offset are included in Cartesian coordinates. After the angle for the inclined axis is

programmed in the NC program, the starting position can be approached (G07) and then the

oblique plunge-cutting (G05) performed.

Job Planning

374

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

Transformations

6.9 Cartesian PTP travel

6.9

Cartesian PTP travel

Function

This function can be used to program a position in a cartesian coordinate system, however,

the movement of the machine occurs in the machine coordinates. The function can be used,

for example, when changing the position of the articulated joint, if the movement runs

through a singularity.

Note

The function can only be used meaningfully in conjunction with an active transformation.

Furthermore, "PTP travel" is only permissible in conjunction with G0 and G1.

Syntax

N... TRAORI

N... STAT='B10' TU='B100' PTP

N... CP

PTP transversal with generic 5/6-axis transformation

If point-to-point transversal is activated in the machine coordinate system (ORIMKS) during an

active generic 5/6-axis transformation with PTP, tool orientation can be programmed both

with rotary axis positions

N... G1 X Y Z A B C

as well as with Euler and/or RPY angle vectors irrespective of the kinematics

N... ORIEULER or ORIRPY

N... G1 X Y Z A2 B2 C2

or the direction vectors

N... G1 X Y Z A3 B3 C3

Both rotary axis interpolation, vector interpolation with large circle interpolation ORIVECT or

interpolation of the orientation vector on a peripheral surface of a taper ORICONxx may be

active.

Non-uniqueness of orientation with vectors

When programming the orientation with vectors, there is non-uniqueness in the rotary axis

positions available. The rotary axis positions to be approached can be selected by

programming STAT = <...>. If

If STAT = 0 is programmed (this is equivalent to the default setting),

the positions which are at the shortest distance from the start positions are approached. If

STAT = 1 is programmed,

the positions which are at a greater distance from the start positions are approached.

Job Planning

376

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

Transformations

6.9 Cartesian PTP travel

Significance

The PTP and CP commands act in a modal manner. CP is the default setting.

If modal applies when programming the STAT value, TU programming is = <...> non-modal.

Another difference is that programming a STAT value only has an effect during vector

interpolation, while programming TU is also evaluated during active rotary axis interpolation.

PTP

point to point (point to point motion)

The movement is executed as a synchronized axis movement; the slowest axis

involved in the movement is the dominating axis for the velocity.

continuous path (path motion)

The movement is executed as Cartesian path motion.

STAT= Position of the articulated joints; this value is dependent on the transformation.

TU=

TURN information acts blockwise. This makes it possible to clearly approach axis

angles between -360 degrees and +360 degrees.

Example

(OERZ XS

(OERZ GRZQ

;

N10 G0 X0 Y-30 Z60 A-30 F10000

Initial setting

→ Elbow up

N20 TRAORI(1)

Transformation on

N30 X1000 Y0 Z400 A0

N40 X1000 Z500 A0 STAT='B10'

Re-orientation without transformation

TU='B100' PTP

→ Elbow down

Job Planning

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

377

Transformations

6.9 Cartesian PTP travel

N50 X1200 Z400 CP

Transformation active again

N60 X1000 Z500 A20

N70 M30

PTP transversal with generic 5-axis transformation

Assumption: This is based on a right-angled CA kinematics.

Program code

Comments

TRAORI

; Transformation CA kinematics on

PTP

; Activate PTP traversing

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 =

; Rotary axis positions C = 270 A = -45

Select clear approach position of rotary axis position:

In block N40, by programming STAT = 1, the rotary axes then travel the long route from their

starting point (C=90, A=90) to the end point (C=270, A=-45), rather than the case would be if

STAT = 0 where they would travel the shortest route to the end point (C=90, A=45).

Description

The commands PTP and CP effect the changeover between Cartesian traversal and traversing

the machine axes.

PTP transversal with generic 5/6-axis transformation

During PTP transversal, unlike 5/6-axis transformation, the TCP generally does not remain

stationary if only the orientation changes. The transformed end positions of all transformation

axes (3 linear axes and up to 3 round axes) are approached in linear fashion without the

transformation still actually being active.

The PTP transversal is deactivated by programming the modal G code CP.

The various transformations are included in the document:

/FB3/ Function Manual Special Functions; Handling Transformation Package (TE4).

Programming the position (STAT=)

A machine position is not uniquely determined just by positional data with Cartesian

coordinates and the orientation of the tool. Depending on the kinematics involved, there can

be as many as eight different and crucial articulated joint positions. These are specific to the

transformation. To be able to uniquely convert a Cartesian position into the axis angle, the

position of the articulated joints must be specified with the command STAT=. The "STAT"

command contains a bit for each of the possible positions as a binary value.

For information about the setting bits to be programmed for "STAT", see:

/FB2/ Description of Functions Extended Functions; Kinematic Transformation (M1),

"Cartesian PTP travel" section.

Job Planning

378

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

Transformations

6.9 Cartesian PTP travel

Programming the axis angle (TU=)

To be able to clearly approach axis angles < ± 360 degrees, this information must be

programmed using the command "TU=".

The axes traverse by the shortest path:

● when no TU is programmed for a position,

● with axes that have a traversing range > ±360 degrees.

Example:

The target position shown in the diagram can be approached in the negative or positive

direction. The direction is programmed under address A1.

A1=225°, TU=Bit 0, → positive direction

A1=-135°, TU=Bit 1, → negative direction

6WDUWLQJ SRVLWLRQ

1HJDWLYH

3RVLWLYH

GLUHFWLRQ

7DUJHW SRVLWLRQ

Example of evaluation of TU for generic 5/6-axis transformation and target positions

Variable TU contains a bit, which indicates the traversing direction for every axis involved in

the transformation. The assignment of TU bits matches the channel axis view of the round

axes. The TU information is only evaluated for the up to 3 possible round axes which are

included in the transformation:

Bit0: Axis 1, TU bit = 0 : 0 degrees <= round axis angle < 360 degrees

Bit1: Axis 2, TU bit = 1 : -360 degrees < round axis angle < 0 degrees

The start position of a round axis is C = 0. By programming C = 270, the round axis travels to

the following target positions:

C = 270: TU bit 0, positive direction of rotation

C = -90: TU bit 1, negative direction of rotation

Job Planning

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

379

Transformations

6.9 Cartesian PTP travel

Further behavior

Mode change

The "Cartesian PTP travel" function is only useful in the AUTO and MDA modes of

operation. When changing the mode to JOG, the current setting is retained.

When the G code PTP is set, the axes will traverse in MCS. When the G code CP is set, the

axes will traverse in WCS.

Power On/RESET

After a power ON or after a RESET, the setting is dependent on the machine data

$MC_GCODE_REST_VALUES[48]. The default traversal mode setting is "CP".

REPOS

If the function "Cartesian PTP travel" was set during the interruption block, PTP can also be

used for repositioning.

Overlaid movements

DRF offset or external zero offset are only possible to a limited extent in Cartesian PTP

travel. When changing from PTP to CP movement, there must be no overrides in the BCS.

Smoothing between CP and PTP motion

A programmable transition rounding between the blocks is possible with G641.

The size of the rounding area is the path in mm or inch, from which or to which the block

transition is to be rounded. The size must be specified as follows:

● for G0 blocks with ADISPOS

● for all the other motion commands with ADIS.

The path calculation corresponds to considering of the F addresses for non-G0 blocks. The

feed is kept to the axes specified in FGROUP(..).

Feed calculation

For CP blocks, the Cartesian axes of the basic coordinate system are used for the

calculation.

For PTP blocks, the corresponding axes of the machine coordinate system are used for the

calculation.

Job Planning

380

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

Transformations

6.9 Cartesian PTP travel

6.9.1

PTP for TRANSMIT

Function

PTP for TRANSMIT can be used to approach G0 and G1 blocks time-optimized. Rather than

traversing the axes of the Basic Coordinate System linearly (CP), the machine axes are

traversed linearly (PTP). The effect is that the machine axis motion near the pole causes the

block end point to be reached much faster.

The part program is still written in the Cartesian workpiece coordinate system and all

coordinate offsets, rotations and frame programming settings remain valid. The simulation on

HMI, is also displayed in the Cartesian Workpiece coordinate system.

Syntax

N... TRANSMIT

N... PTPG0

N... G0

N... G1 ...

Significance

TRANSMIT Activates the first declared TRANSMIT function

(see section "Milling on turned parts: TRANSMIT")

PTPG0

Point to Point G0 (point-to-point motion automatic at each G0 block and then

set CP again)

Because STAT and TU are modal, the most recently programmed value

always acts.

PTP

point to point; (point to point motion)

For TRANSMIT, PTP means that in the Cartesian spirals will be retracted to

Archimedean spirals either about the pole or from the pole. The resulting tool

motions run significantly different as for CP and are represented in the

associated programming examples.

STAT=

Resolving the non-uniqueness with regard to the pole.

TU=

TU is not relevant for PTP with TRANSMIT

Job Planning

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

381

Transformations

6.9 Cartesian PTP travel

Example of the retraction from the pole with PTP and TRANSMIT

PTP

N070 X20 Y2

N060 X0 Y0

-30

-20

-10

-20

-30

N050 X10 Y0

Programming

Comments

N001 G0 X90 Z0 F10000 T1 D1 G90

; Initial setting

N002 SPOS=0

N003 TRANSMIT

; Transformation TRANSMIT

N010 PTPG0

; For each G0 block, automatically

PTP followed by CP

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

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

383

Transformations

6.9 Cartesian PTP travel

Description

PTP and PTPG0

PTPG0 is considered for all transformations that can process PTP. PTPG0 is not relevant is all

other cases.

G0 blocks are processed in CP mode.

The selection of PTP or PTPG0 is performed in the parts program or by the deselection of CP

in the machine data $MC_GCODE_RESET_VALUES[48].

CAUTION

Restrictions

With regard to tool motions and collision, a number of restrictions and certain function

exclusions apply, such as:

no tool radius compensation (TRC) may be active with PTP.

With PTPG0 , for active tool radius compensation (TRC), is traversed by CP.

PTP does not permit smooth approach and retraction (SAR).

With PTPG0, CP traversal is used for smooth approach and retraction (SAR).

PTP does not permit cutting cycles (CONTPRON, CONTDCON).

With PTPG0 cutting cycles (CONTPRON, CONTDCON) are traversed by CP.

Chamfer (CHF, CHR) and rounding (RND, RNDM) are ignored.

Compressor is not compatible with PTP and will automatically be deselected in PTP

blocks.

An axis superimposing in the interpolation may not change during the PTP section.

If G643 is specified, an automatic switch to G642 is made after smoothing with axial

accuracy.

For active PTP, the transformation axes cannot be simultaneously positioning axes.

References:

/FB2/ Function Manual Extended Functions; Kinematic Transformation (M1),

"Cartesian PTP travel" section

PTP for TRACON:

PTP can also be used with TRACON, provided the first chained transformation supports PTP.

Meaning of STAT= and TU= for TRANSMIT

If a rotary axis is to turn by 180 degrees or the contour for CP passes through the pole,

rotary axes depending on the machine data $MC_TRANSMIT_POLE_SIDE_FIX_1/2 [48] can be

turned by -/+ 180 degrees and traversed in clockwise or counter-clockwise direction. It can

also be set whether traversal is to go through the pole or whether rotation around the pole is

to be performed.

Job Planning

384

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

Transformations

6.10 Constraints when selecting a transformation

6.10

Constraints when selecting a transformation

Function

Transformations can be selected via a parts program or MDA. Please note:

● No intermediate movement block is inserted (chamfer/radii).

● Spline block sequences must be excluded; if not, a message is displayed.

● Fine tool compensation must be deselected (FTOCOF); if not a message is displayed.

● Tool radius compensation must be deselected (G40); if not a message is displayed.

● An activated tool length offset is included in the transformation by the control.

● The control deselects the current frame active before the transformation.

● The control deselects an active operating range limit for axes affected by the

transformation (corresponds to WALIMOF).

● Protection zone monitoring is deselected.

● Continuous path control and rounding are interrupted.

● All the axes specified in the machine data must be synchronized relative to a block.

● Axes that are exchanged are exchanged back; if not, a message is displayed.

● A message is output for dependent axes.

Tool change

Tools may only be changed when the tool radius compensation function is deselected.

A change in tool length offset and tool radius compensation selection/deselection must not

be programmed in the same block.

Frame change

All statements, which refer exclusively to the base coordinate system, are permissible

(FRAME, tool radius compensation). However, a frame change with G91 (incremental

dimension) - unlike with an inactive transformation - is not handled separately. The

increment to be traveled is evaluated in the workpiece coordinate system of the new frame -

regardless of which frame was effective in the previous block.

Exceptions

Axes affected by the transformation cannot be used

● as a preset axis (alarm),

● for approaching a checkpoint (alarm),

● for referencing (alarm).

Job Planning

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

385

Transformations

6.11 Deselect transformation (TRAFOOF)

6.11

Deselect transformation (TRAFOOF)

Function

The TRAFOOF command deactivates all active transformations and frames.

Note

Frames required after this must be activated by renewed programming.

Please note:

The same restrictions as for selection are applicable to deselecting the transformation (see

section "Constraints when selecting a transformation").

Syntax

TRAFOOF

Significance

TRAFOOF

Command for deactivating all active transformations/frames

Job Planning

386

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

Transformations

6.12 Chained transformations (TRACON, TRAFOOF)

6.12

Chained transformations (TRACON, TRAFOOF)

Function

Two transformations can be chained so that the motion components for the axes from the

first transformation are used as input data for the chained second transformation. The motion

parts from the second transformation act on the machine axes.

The chain may include two transformations.

Note

A tool is always assigned to the first transformation in a chain. The subsequent

transformation then behaves as if the active tool length were zero. Only the basic tool

lengths set in the machine data (_BASE_TOOL_) are valid for the first transformation in the

chain.

Machine manufacturer

Take note of information provided by the machine manufacturer on any transformations

predefined by the machine data.

Transformations and chained transformations are options. The current catalog always

provides information about the availability of specific transformations in the chain in specific

controls.

Applications

● Grinding contours that are programmed as a side line of a cylinder (TRACYL) using an

inclined grinding wheel, e.g., tool grinding.

● Finish cutting of a contour that is not round and was generated with TRANSMIT using

inclined grinding wheel.

Syntax

TRACON(trf,par)

This activates a chained transformation.

TRAFOOF

Job Planning

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

387

Transformations

6.12 Chained transformations (TRACON, TRAFOOF)

Significance

TRACON

This activates the chained transformation. If another transformation was

previously activated, it is implicitly disabled by means of TRACON().

TRAFOOF

The most recently activated (chained) transformation will be disabled.

trf

Number of the chained transformation:

0 or 1 for first/single chained transformation.

If nothing is programmed here, then this has the same meaning as

specifying value 0 or 1, i.e., the first/single transformation is activated.

2 for the second chained transformation. (Values not equal to 0 - 2

generate an error alarm).

par

One or more parameters separated by a comma for the transformations in

the chain expecting parameters, for example, the 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 parameters 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 trf. For example: TRACON( , 3.7).

Requirements

The second transformation must be "Inclined axis" (TRAANG). The first transformation can be:

● Orientation transformations (TRAORI), including universal milling head

● TRANSMIT

● TRACYL

● TRAANG

It is a condition of using the activate command for a chained transformation that the

individual transformations to be chained and the chained transformation to be activated are

defined by the machine data.

The supplementary conditions and special cases indicated in the individual transformation

descriptions are also applicable for use in chained transformations.

Information on configuring the machine data of the transformations can be found in:

/FB2/ Function Manual Extended Functions; Kinematic Transformations (M1) and

/FB3/ Function Manual, Special Functions; 3- to 5-Axis Transformations (F2).

Job Planning

388

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

Tool offsets

7.1

Offset memory

Function

Structure of the offset memory

Every data field can be invoked with a T and D number (except "Flat D No."); in addition to

the geometrical data for the tool, it contains other information such as the tool type.

Flat D number structure

The "Flat D No. structure" is used if tool management takes place outside the NCK. In this

case, the D numbers are created with the corresponding tool compensation blocks without

assignment to tools.

T can continue to be programmed in the part program. However, this T has no reference to

the programmed D number.

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.

¹Also applies to milling tools for 3D face milling

²Tool type for slotting saw

³Reserved: Is not used by SINUMERIK 840D

Job Planning

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

389

Tool offsets

7.1 Offset memory

Tool parameter

Meaning of system variables

Remarks

number (DP)

$TC_DP1

Tool type

For overview see list

$TC_DP2

Tool nose 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_DP6¹

Radius 1 / length 1

Milling/turning/grinding tool

$TC_DP6²

diameter d

Slotting saw

$TC_DP7¹

Length 2 / corner radius, tapered milling tool

Milling tools

$TC_DP7²

Slot width b corner radius

slotting saw

$TC_DP8¹

Rounding radius 1 for milling tools

Milling tools

$TC_DP8²

projecting length k

slotting saw

$TC_DP9^1.3

Rounding radius 2

Reserved

$TC_DP10¹

Angle 1 face end of tool

Tapered milling tools

$TC_DP11¹

Angle 2 tool longitudinal axis

Tapered milling tools

Wear

Length and radius compensation

$TC_DP12

Length 1

$TC_DP13

Length 2

$TC_DP14

Length 3

$TC_DP15¹

Radius 1 / length 1

Milling/turning/grinding tool

$TC_DP15²

diameter d

slotting saw

$TC_DP16¹

Length 2 / corner radius, tapered milling tool,

Milling tools

$TC_DP16³

slot width b corner radius

slotting saw

$TC_DP17¹

Rounding radius 1 for milling tools

Milling / 3D face milling

$TC_DP17²

projecting length k

slotting saw

$TC_DP18^1.3

Rounding radius 2

Reserved

$TC_DP19¹

Angle 1 face end of tool

Tapered milling tools

$TC_DP20¹

Angle 2 tool longitudinal axis

Tapered milling tools

Tool base dimension/

Tool length offsets

adapter

$TC_DP21

Length 1

$TC_DP22

Length 2

$TC_DP23

Length 3

Technology

$TC_DP24

Clearance angle

only for turning tools

$TC_DP25

Reserved

Comments

Several entry components are available for geometric variables (e.g. length 1 or radius).

These are added together to produce a value (e.g., total length 1, total radius), which is then

used for the calculations.

Offset values not required must be assigned the value zero.

Job Planning

390

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

Tool offsets

7.1 Offset memory

Tool parameters $TC-DP1 to $TC-DP23 with contour tools

Note

The tool parameters not listed in the table, such as $TC_DP7, are not evaluated, i.e. their

content is meaningless.

Tool parameter number

Significance

Cutting Dn

Remarks

(DP)

$TC_DP1

Tool type

400 ... 599

$TC_DP2

Tool nose position

Geometry

Length compensation

$TC_DP3

Length 1

$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 compensations

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, 03/2010, 6FC5398-2BP20-1BA0

391

Tool offsets

7.2 Additive offsets

7.2

Additive offsets

7.2.1

Selecting additive offsets (DL)

Function

Additive offsets can be considered as process offsets that can be programmed in the

machining. They refer to the geometrical data of a cutting edge and are therefore a

component of tool cutting data.

Data of an additive offset are addressed using a DL number (DL: Locationdependent; offsets

regarding the location of use) and entered via the operator interface.

Application

Dimension errors caused be the location of use can be compensated using additive offsets.

Syntax

DL=<number>

Significance

Command to activate an additive offset

The additive tool offset data to be activated is specified using the <number>

parameter.

Note

The machine data is used to define the number of additive offsets and also activate them

(→ carefully observe the machine OEM's data!).

Job Planning

392

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

Tool offsets

7.2 Additive offsets

Example

The same cutting edge is used for 2 bearing seats:

/RFDWLRQ RI XVH

;

' '/

Program code

Comments

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 position.

Job Planning

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

393

Tool offsets

7.2 Additive offsets

7.2.2

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

Function

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

System variable

Significance

$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

parameter 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

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

Job Planning

394

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

Tool offsets

7.2 Additive offsets

7.2.3

Delete additive offsets (DELDL)

Function

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>]

Significance

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).

Delete status

Value: Significance:

Deletion was successfully completed.

Offsets have not been deleted (if the parameter settings

specify exactly one tool edge), or not deleted completely (if

the parameter settings specify several cutting edges).

Note

Wear and setting-up values of active tools cannot be deleted (essentially the same as the

delete behavior of D or tool data).

Job Planning

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

395

Tool offsets

7.3 Special handling of tool offsets

7.3

Special handling of tool offsets

Function

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).

More information on summed offsets, refer to:

References:

Function Manual, Tool Management

Setting data

Setting Data

Significance

SD42900 $SC_MIRROR_TOOL_LENGTH

Mirroring of tool-length components and

components of the tool base dimension.

SD42910 $SC_MIRROR_TOOL_WEAR

Mirroring of wear values of the tool-length

components.

SD42920 $SC_WEAR_SIGN_CUTPOS

Evaluating the sign of the wear components as

a function of the tool nose 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

geometry axes.

SD42950 $SC_TOOL_LENGTH_TYPE

Assignment of the tool length components

independent of tool type.

SD42960 $SC_TOOL_TEMP_COMP

Temperature compensation value in tool

direction. Also operative when tool orientation is

programmed.

References

Function Manual Basic Functions; Tool Offset (W1)

Job Planning

396

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

Tool offsets

7.3 Special handling of tool offsets

Further Information

Activation of modified setting data

When the setting data described above are 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 are to be reevaluated, the tool must be selected again.

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 have 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.

Job Planning

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

397

Tool offsets

7.3 Special handling of tool offsets

7.3.1

Mirroring of tool lengths

Function

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.

;

:&6

' ZLWK 6/

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.

Job Planning

398

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

Tool offsets

7.3 Special handling of tool offsets

7.3.2

Wear sign evaluation

Function

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 tool nose position (turning and grinding tools, tool types 400), then

the sign evaluation of the wear components in the machining plane depends on the tool nose

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

position.

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

zero), are designed using an X:

Tool nose position

Length 1

Length 2

Note

The sign evaluation using SD42920 and SD42910 are independent of one another. If e.g.

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

remains unchanged.

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".

Job Planning

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

399

Tool offsets

7.3 Special handling of tool offsets

7.3.3

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

TOWWCS, TOWBCS, TOWTCS, TOWKCS)

Function

Depending on the kinematics of the machine or the availability of an orientable toolholder,

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 can produce tool length offsets that can be used to

incorporate the tool length component "wear" into an active tool via the corresponding G

code 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

Significance

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 of tool length at toolholder reference point (orientable toolholder)

TOWKCS

Offsets of tool length at tool head (kinematic transformation)

Job Planning

400

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

Tool offsets

7.3 Special handling of tool offsets

Further Information

Distinguishing features

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

G code

Wear value

Active orientable toolholder

TOWSTD

Initial value, tool length

Wear values are subject to rotation.

TOWMCS

Wear value in MCS. TOWMCS is

It only rotates the vector of the

identical to TOWSTD if a tool holder

resultant tool length without taking

that can be orientated is not active.

into 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

TOWMCS without taking into account

system.

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 toolholder

If neither a kinematic transformation nor an orientable toolholder 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)

Job Planning

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

401

Tool offsets

7.3 Special handling of tool offsets

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

should be subject to a rotation using adapter transformation or a tool holder that can be

orientated if one of the following G codes is active:

● TOWSTD Default setting

For offsets in the tool length

● TOWMCS wear values

In the machine coordinate system (MCS)

● TOWWCS wear values

In the workpiece coordinate system (WCS)

● TOWBCS wear values (BCS)

In the basic coordinate system

● TOWTCS wear values in the tool coordinate system at the tool holder reference (T tool

holder reference)

● TOWKCS Wear values in the coordinate system of the tool head for kinematic transformation

Note

Evaluation of individual wear components (assignment to geometry axes, sign evaluation)

is influenced by:

• The active plane

• The adapter transformation

• Following setting data:

- SD42910 $SC_MIRROW_TOOL_WEAR

- SD42920 $SC_WEAR_SIGN_CUTPOS

- SD42930 $SC_WEAR_SIGN

- SD42940 $SC_TOOL_LENGTH_CONST

- SD42950 $SC_TOOL_LENGTH_TYPE

Job Planning

402

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

Tool offsets

7.3 Special handling of tool offsets

7.3.4

Tool length and plane change

Function

When setting data SD42940 $SC_TOOL_LENGTH_CONST is set not equal to zero, then

you can assign the tool length components - such as lengths, wear and basic dimension - to

the geometry axes for turning and grinding tools when changing the plane.

SD42940 $SC_TOOL_LENGTH_CONST

Setting data not equal to zero:

The assignment of tool length components (length, wear and tool base dimension) to

geometry axes does not change when the machining plane is changed (G17 - G19).

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

turning and grinding tools (tool types 400 to 599):

Content

Length 1

Length 2

Length 3

-17

-18

-19

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

-17

-18

-19

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

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

403

Tool offsets

7.4 Online tool offset (PUTFTOCF, FCTDEF, PUTFTOC, FTOCON, FTOCOF)

7.4

Online tool offset (PUTFTOCF, FCTDEF, PUTFTOC, FTOCON,

FTOCOF)

Function

When the "Online tool offset" function is active, a tool length offset resulting from the

machining is applied immediately on grinding tools.

An application example is CD dressing, where the grinding wheel is dressed in parallel to

machining.

'UHVVLQJ UROO

'UHVVLQJ DPRXQW

*ULQGLQJ GLVF

OHQJWK

WR EH

FRUUHFWHG

:RUNSLHFH

The tool length offset can be changed from the machining channel or a parallel channel

(dresser channel).

The online tool offset is written using various functions dependent on the timing of the

dressing process:

● Continuous write, non-modal (PUTFTOCF)

With PUTFTOCF, dressing is carried out at the same time as machining.

The tool offset is changed continuously in the machining channel according to a

polynomial function of the first, second or third order, which must have been defined

previously with FCTDEF.

PUTFTOCF is always non-modal; in other words, it takes effect in the subsequent traversing

block.

● Continuous write, modal: ID=1 DO FTOC (see "Online tool offset (FTOC) (Page 593)")

● Discrete write (PUTFTOC)

With PUTFTOC, dressing is not carried out at the same time as machining from a parallel

channel. The offset value specified with PUTFTOC takes effect immediately in the

destination channel.

Note

Online tool offset can be applied only to grinding tools.

Job Planning

404

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

Tool offsets

7.4 Online tool offset (PUTFTOCF, FCTDEF, PUTFTOC, FTOCON, FTOCOF)

Syntax

Activate/deactivate online tool offset in the destination channel:

FTOCON

FTOCOF

Write online tool offset:

● Continuous, non-modal:

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

PUTFTOCF(<function>,<reference value>,<tool parameter>,<channel>,<spindle>)

● Discrete:

PUTFTOC(<offset value>,<tool parameter>,<channel>,<spindle>)

Significance

FTOCON:

Activate online tool offset

FTOCON must be written in the channel in which the online tool offset is to

take effect.

FTOCOF:

Cancel online tool offset

With FTOCOF, the offset is no longer applied; however, the complete value

written with PUTFTOC is corrected in the cutting-edge-specific offset data.

Note:

In order to definitively deactivate the online tool offset, the tool (T...) still

needs to be selected/deselected after FTOCOF.

FCTDEF:

FCTDEF is used to define the polynomial function for PUTFTOCF.

Parameter:

<function>:

Number of the polynomial function

Type: INT

<LLimit>:

Lower limit value

Type: REAL

<ULimit>:

Upper limit value

Type: REAL

<a0> ... <a3>:

Coefficients of polynomial function

Type: REAL

Job Planning

Programming Manual, 03/2010, 6FC5398-2BP20-1BA0

405

SINUMERIK 840D sl/828D. Job Planning. Programming Manual (2010-2018) - page 19