SINUMERIK 840D sl. Training. Operate - Turning (2016-2020)

General information on workpiece production

2.10

2.10.3 Simultaneous recording

In Automatic mode, i.e. during the program execution on the machine, the tool movements can

be simultaneously recorded in the top view, the three-side view or in the 3D view (with the 3D

simulation option). This option is especially useful when the working area of the machine cannot

be viewed clearly. During simultaneous recording, similar functions are available as for

simulation.

Activating simultaneous recording:

X Before starting the NC program, press the Sim. rec. softkey

X The execution of the program is simultaneously recorded after pressing CYCLE START. You

can display the tool paths and the workpiece machining in parallel to the machining.

→ Top view

→ 3D view

→ Side views

→ Zoom, magnify,

turn, cut

→ Displaying the

tool

General information on workpiece production

2.11

Executing programs (AUTOMATIC)

SINUMERIK Operate provides functions that support the workflow during the execution of mold-

making programs.

2.11.1 Display all relevant mold-making functions

→ Active

G functions

→ M functions

→ Basic blocks

→ Running time,

→ Program levels

→ All

G functions

Selection of the various displays during the execution:

Active G and M functions of up to 16 G groups.

Basic blocks, running time and workpiece counters

Program level for nested subprogram calls

Current position and distance-to-go display to the target position

All relevant G code functions for mold-making (Advanced Surface) can be displayed via the

expanded softkey bar with the All G functions softkey. The G functions are color coded, e.g.

CTOL, OTOL for the tolerances.

General information on workpiece production

2.11

2.11.2 Program running time

To gain an overview of the program running time and the number of machined workpieces, use

the Times/counters functions

Pressing the softkey the first time shows how long the program has already been running

. At

every further start of the program, the time required to run the entire program the first time and

the remaining time are displayed

. In addition, you can follow how much of the current

program has been completed in percent on a progress bar

The running times can be displayed block-by-block/non-modally and saved

. The running

times determined by the simulation are shown with a blue backg8round. After the first processing,

the actually determined times are shown with a green backg8round. The Settings softkey is used

to configure whether the running times should be displayed and saved.

When a program is executed for the first time, its progress is estimated based on the program

size and the actual program offset; this means it can differ from the actual running time.

General information on workpiece production

2.11

2.11.3 Handwheel override

In the AUTOMATIC mode, while executing a program, small compensations and override feed of

the tool in the tool direction are possible using a handwheel. When the orientation of the tool

changes, the handwheel override that has been accumulated is also rotated. The manual

compensation acts as override to the traversing motions from the NC program.

Handwheel override

Override with handwheel:

Handwheel override of axes

(DRF offset)

Handwheel override in the tool direction

(TOFFON function)

Traverse axes in increments only

Active in the following states:

NC/CYCLE stop

Single block mode

Override 0% and higher

Programmed STOP M0

A typical application is, for example, changing

the swivel head position (rotary axes) or the

infeed depth in the tool direction, in order for

example to mill a workpiece with tolerance.

Activating override

X In AUTOMATIC mode, press the Program control softkey

and activate DRF handwheel

offset

Displaying override

X Open the expanded softkey bar >>

and then the Overrides softkey

General information on workpiece production

2.11

2.11.4 Block search

You can perform a block search in the Reset machine state. The program data is prepared in

such a way that all relevant parameters (tool, zero offsets, M functions, etc.) are available when

accessing the program.

Possible search variants:

Precise return to the point of interruption, even after power off

To any CNC block in the DIN/ISO programs

To any subprogram levels in DIN/ISO programs

Machining step programs and position patterns in ShopMill

Accelerated block search in large mold-making programs

To use the block search:

X The block search can be configured individually using the Search mode softkey

e.g. with

and without calculation or with/without approach.

X Using the Interruption point softkey

a jump is made to the last executed line of the NC

program.

X Using the Search pointer

you can define the search target within an NC program,

e.g. specific line number, mark or text.

X Start search

performs the search; CYCLE START executes the program at the search

location.

General information on workpiece production

2.12

Collision avoidance

The improved collision avoidance available in three variants on the control prevents the collision

of moving machine components with static components; it is active in setup operation and in

automatic operation.

Collision avoidance is based on a machine model. The kinematics of the machine are described

as a kinematic chain. Protection areas are attached to these chains for the protected machine

parts. The geometry of the protection areas is defined using protection area elements. Protection

areas are, for example, spindles, tools, tool table and machine covers.

The "Collision avoidance" function regularly calculates the clearance from these protection

areas. When two protection areas approach one another and a specific safety clearance is

reached, an alarm is displayed and the program is stopped before the corresponding traversing

block and/or the traversing motion is stopped.

General information on workpiece production

2.12

Overview of the Collision Avoidance variants

Collision Avoidance ECO

Collision Avoidance

Collision Avoidance ADVANCED

Components / protection areas are

Includes Collision Avoidance ECO

In addition, tools and workpiece

described with simple geometric

material removal for collision

More protection area elements

bodies.

monitoring are considered.

Components/elements are modeled

The collision locations are

Further software from third-parties

as STL files.

visualized directly from the CNC

on an external PC in real-time is

X The collision of moving machine

user interface.

used to match position values,

components with static components

setup data and tool geometries (e.g.

X The collision of moving machine

is prevented thanks to the more

ModulWorks Corp.).

components with static components

exact geometry description of the

is prevented, e.g. spindle with the

X Machine, tool and workpiece are

components.

machine covers.

protected dynamically.

Important functions for 3- to 5-axis machining

3.1

Introduction

Especially within the context of mold-making machining, the entire CAD/CAM/CNC process

chain plays a major role in terms of ensuring optimum results on the machine.

The CAD system generates the geometry of the desired workpiece. Based on this geometry file,

the CAM system generates the corresponding machining strategy with the associated

technology information.

The data format output from the CAM system is generally an APT or CL data file. This is

converted into an executable NC code in the postprocessor.

The upstream postprocessor must support the programmable functions of the SINUMERIK

control in order to use the performance capability of SINUMERIK controls to the full.

The postprocessor should ensure that the higher-order functions of SINUMERIK controls (as

described in this section) are activated in the best possible way. An overview of all higher-order

SINUMERIK functions is provided in the following sections.

CAD

CAM

CNC

(Design)

(NC Programming)

(Machining)

Geometry

Tool path

NC program

Workpiece

APT source

Important functions for 3- to 5-axis machining

3.2

Explanation of the terms: swivel, frames and

TRAORI

The swivel (CYCLE800) and TRAORI features can be used to control rotary axes and angle the

tool in relation to the machining surface. During swiveling, the rotary axes are positioned once

and the linear axes X, Y, Z move during machining. The tool is oriented from a start position

through to an end position and will then only work with the three linear axes. It is aligned in

relation to the surface by means of a static process.

In contrast to swiveling, TRAORI is a dynamic process. The rotary and linear axes can be

traversed simultaneously during machining. The orientation of the tool in space can be changed

continuously. All axes (rotary and linear axes) are interpolated at the same time.

Frames affect only the coordinate system and only the coordinate system is modified,

for example, rotated, scaled or moved. CYCLE800 takes the machine kinematics into account

during swiveling, i.e. attention is paid to tool compensations and zero points. In the case of

frames (e.g. ROT), these must be taken into account by the user.

Frames

The frame is a self-contained arithmetic rule

that transforms one Cartesian coordinate

system into another Cartesian coordinate

system.

In the example, the coordinate system is twice

subjected to translatory movement. This is the

case, for example, if you set the zero point at

the corner of the workpiece by means of zero

offset.

Swivel

The tool is aligned with the machining surface

by moving the rotary axes. This example

involves rotation of rotary axis B

and the

tool is positioned in relation to the XY plane

. Machining then takes place in this plane.

Important functions for 3- to 5-axis machining

3.3

TRAORI

The tool is aligned with the machining surface

dynamically during the milling process by

means of linear and rotary axis interpolation.

The tool length is taken into account and the

kinematic compensatory movements are

initiated by the TRAORI function when the

rotary axes are rotated.

3.3

Transforming coordinate systems - Frames

Coordinate systems

Machine coordinate system

with reference

point and zero offset (G54, G55, etc.) are

familiar terms.

Using frames, the coordinate systems can be

shifted, rotated, mirrored and scaled so that

they can be aligned with any workpiece

surface. This allows the programming

overhead to be reduced to a minimum.

With frames, starting from the current

workpiece coordinate system

, the position

of a target coordinate system is defined by

specifying coordinates and angles.

Possible frames include

Basic frame (basic offset, G500)

Settable frames (G54, G55, etc.)

Programmable frames (TRANS, ROT,

etc.)

Using frames it is possible to machine surfaces that can be shifted and rotated in space as

required. All subsequent traversing commands now relate to the new workpiece coordinate

system shifted using frames.

Important functions for 3- to 5-axis machining

3.4

Swivel - CYCLE800

Function

You can use swivel heads or swivel tables to set up and machine inclined planes. Swiveling is

possible in JOG mode and AUTOMATIC mode. Swivel operation parameter assignment and

programming are facilitated by the clearly laid out graphics. You can either program all the swivel

axes directly on the machine (A, B, C) or you can simply specify the rotations around the

geometry axes (X, Y, Z) of the workpiece coordinate system as described in the relevant

workpiece drawing. The rotation of the workpiece coordinate system in the program is then

automatically converted to a rotation of the relevant swivel axis of the machine during machining.

The swivel axes are always rotated in such a way that the machining plane is perpendicular to

the tool axis for machining. The machining plane then remains fixed during machining.

When the axes are swiveled, the active zero points and tool compensations are automatically

converted for the swiveled state; this results in a new coordinate system.

Machine kinematics

Swivel head

Swivel table

Swivel head + swivel table

(type T)

(type P)

(type M)

Swiveling tool carrier

Swiveling workpiece holder

Mixed kinematics

Important functions for 3- to 5-axis machining

3.4

Procedure for programming swivel movement and subsequent machining:

X Swivel the coordinate system into the plane to be machined.

X Program the machining process as usual in the X/Y plane.

X Swivel the coordinate system back to its original position.

Basic procedure for using the swivel cycle

X Call the Swivel function in the program.

X Select the name of the swivel data record

X Select "yes" for swivel if you wish to perform a swivel movement. Select "new" as swivel

movement if you wish to perform a new swivel movement, or "additive" if you wish to base the

movement on a previous swivel movement

X Specify the reference point before rotation (X0, Y0, Z0)

X Select the "axis-by-axis" swivel mode directly or via the projection angle

X Enter the angle through which the axis should swivel. In the axis-by-axis mode, you can enter

the angle for each axis

X Shift the zero point on the swiveled plane

Important functions for 3- to 5-axis machining

3.4

Example program for swiveling in programGUIDE

Standard milling and drilling cycles are applied to swiveled machining surfaces in the following

example.

X Face milling of the workpiece.

X Swiveling the machining plane by X=-15 degrees and milling a circular pocket.

X Swiveling by Y=-7 or +7 degrees, face grooving with milling cutter for the holes and creating

two holes at angles of +7 degrees and two holes at -7 degrees.

N100

; Swivel the plane to the basic position

N110

CYCLE800(4,"TABLE",200000,57,0,0,0,0,0,0,0,0,0,1,,1)

N120

; Raw part definition for simulation

N130

WORKPIECE(,,,"BOX",112,0,51,-80,-2.5,-2.5,102.5,102.5)

N140

T10 D1; T="CUTTER_D32"

N150

M06

N160

S5000 M03

N170

G0 G54 X0 Y0

N180

TRANS Z50 ;Zero offset in Z workpiece upper edge

N190

;Face milling of workpiece in basic position

N200

CYCLE61(10,1,5,0,0,0,100,100,1,20,0,2000,32,0,1,0)

N210

;Swiveling into the plane_1 X=-15 DEGREES

N220

CYCLE800(4,"TABLE",200000,57,0,0,50,-15,0,0,0,0,0,1,,1)

N230

;Face milling of workpiece in Plane_1

Important functions for 3- to 5-axis machining

3.4

N240

CYCLE61(35,25.8,5,0,0,0,100,103.6,5,20,0.2,2000,31,0,1,0)

N250

T11 D1; T="CUTTER_D16"

N260

M06

N270

S8000 M03

N280

G54 X50 Y51.76 M08; Pre-position on center of pocket

N290

; Circular pocket roughing and finishing Plane_1

N300

POCKET4(10,0,2,-

15,40,50,51.76,5,0.1,0.1,2000,2000,0,21,80,0,,10,2.5,0,,,10100,111,10)

N310

POCKET4(10,0,2,-

15,40,50,51.76,15,0.1,0.1,1000,1000,0,22,80,0,,5,2.5,0,,,10100,111,10)

N320

T12 D1; T="CUTTER_D10"

N330

M06

N340

S6000 M03 F500

N350

G54 X0 Y0 M08

N360

; Calculate swiveling Plane_1 with new center point X1, Y1 X=-15 degrees

N370

CYCLE800(4,"TABLE",220000,57,0,0,50,-15,0,0,50,51.76,0,0,,1)

N380

; Swiveling Plane_1 additive Y=-7 degrees

N390

CYCLE800(4,"TABLE",200001,57,-35,-24,0,0,-7,0,0,0,0,1,,1))

N400

; Area -7 degrees with milling cutter face grooving so that the drill inserts vertically later

N410

MCALL CYCLE82(10,0,5,-3,,1,0,1,12)

N420

G0 X0 Y0 M8

N430

X0 Y60

N440

MCALL

N450

; Calculate swiveling Plane_1 with new center point X1, Y1 X=-15 degrees

Important functions for 3- to 5-axis machining

3.4

N460

N141 CYCLE800(4,"TABLE",220000,57,0,0,50,-15,0,0,50,51.76,0,0,,1)

N465

; Swiveling Plane_1 additive Y=+7 degrees

N470

CYCLE800(4,"TABLE",200001,30,35,-24,0,7,0,0,0,0,0,1,,1)

N480

; Surface +7 degrees with milling cutter face grooving so that the drill later inserts

vertically

N490

MCALL CYCLE82(10,0,5,-3,,1,0,1,12)

N500

G0 X0 Y0 M8

N510

X0 Y60

N520

MCALL

N530

T13 D1; T="DRILL_D8.5"

N540

N550

S4000 M3 F500 D1

N560

G54 G0 X0 Y0 M8

N570

; Deep-hole drilling D8.5 Y=+7 degrees

N580

MCALL CYCLE83(10,0,2,-20,,-5,,054,0,100,0,0,4,1,0,0,0,1,11121112)

N590

G0 X0 Y0

N600

X0 Y60

N610

MCALL

N615

; Calculate swiveling Plane_1 with new center point X1, Y1 X=-15 degrees

Important functions for 3- to 5-axis machining

3.4

N620

CYCLE800(4,"TABLE",220000,57,0,0,50,-15,0,0,50,51.76,0,0,,1)

N625

; Swiveling Plane_1 additive Y=-7 degrees

N630

CYCLE800(4,"TABLE",200001,54,-35,-24,0,-7,0,0,0,0,0,1,,1)

N640

; Deep-hole drilling D8.5 with -7 degrees

N650

MCALL CYCLE83(10,0,2,-20,,-5,,054,0,100,0,0,4,1,0,0,0,1,11121112)

N660

G0 X0 Y0

N670

X0 Y60

N680

MCALL

N690

; Swivel the plane to the basic position

N700

CYCLE800(2,"TABLE",200000,57,0,0,0,0,0,0,0,0,0,1,,1)

N710

; Deselection CYCLE800

N720

CYCLE800()

N730

M30; end of program

Important functions for 3- to 5-axis machining

3.5

TRAORI 5-axis transformation

Inclined planes can be machined with the aid of CYCLE800. The tool is inclined relative to the

workpieces so that inclined workspaces can be machined. The inclination is performed at the

start of the machining and is not changed during the machining of the inclined plane. However, in

many case this static inclined position is not sufficient. A constantly changing tool orientation

relative to the workpiece is required. So that this can be performed in a clear and user-friendly

way, the 5-axis transformation, which is activated by the TRAORI command, has been

introduced.

3.5.1

Basics of simultaneous 5-axis machining

The various kinematics of 5-axis machines were described in Section 1.5. A distinction is made

between three basic types.

Machines with a rotatable tool which is swiveled by means of two rotary axes.

Machines with a rotatable workpiece which is swiveled while the orientation of the tool

remains fixed in space.

Machines of the "mixed" type on which one rotary axis rotates the tool and the second rotary

axis swivels the workpiece.

Machine kinematics and machine movement

Motion sequence for head/head kinematics

Motion sequence for table/table kinematics

A semicircle must be described in the X/Y

At the start, the A axis must be rotated through

plane for one cycle. At the same time, the tool

90°. The tool is then perpendicular to the

must be rotated through 180° around Z if the

surface. For one cycle, the C axis swivels from

tool is always to be perpendicular to the

+90° to -90°. Therefore, for one cycle (a

surface. Therefore, for the machining of one

semicircle), only the C axis moves.

cycle, 3 axes, X, Y and C must move.

It is clear from the example that totally different machine movements produce the same

machining result. If we look at the movements more exactly, we can see that in both cases the

movement of the tool tip on the workpiece and the tool orientation relative to the surface are

identical.

Important functions for 3- to 5-axis machining

3.5

Effect of the tool length on the machine movement

To investigate the effect of the tool length on the machine movement, let us consider a further

example. The base circle of the half sphere shown in the graphic is to be machined with an

inclined tool.

In the graphic, you can see that different tool

lengths result in different machine

movements. To machine the circle on the

lower part of the half sphere, traversing must

be performed in a circle in the X-Y plane and

also the C axis must be rotated through 360°

during the circular movement. Whereas the

circle for the tool tip always remains the same

size irrespective of the tool length, the circle

that the machine axes must describe

increases with the tool length. This is indicated

by the two red circles that are produced with

different tool lengths.

It is clear that when programming machine

axis positions, a different program must be

created for each tool length, while the

movement of the tool tip always remains the

same.

Rotary axis movement and tool orientation

The rotary axes in 5-axis machines are used to enable the various orientations of the tool relative

to the workpiece. The movement of a rotary axis normally not only changes the tool orientation,

but also the position of the tool tip in relation to the workpiece surface if this is not prevented by a

suitable mechanism.

Tool tip moves

Tool tip fixed in space

Example

shows that the movement of the A axis not only changes the tool orientation to the

workpiece. At the same time, the tool tip moves in space, a circular path in the Z-X plane in our

example. This is an unwanted side effect.

Generally, the movement shown in

is desirable, in which compensatory movements of the

linear axes ensure that the tool tip is fixed in space during rotary axis movements.

Important functions for 3- to 5-axis machining

3.5

Simultaneous movement of linear/rotary axes

This effect is also shown during simultaneous movement of linear and rotary axes.

The graphic shows the simultaneous

movement of the A axis and the Y axis. In

situation

, both axes move synchronously;

they are interpolated linearly with one another.

A straight path of machine axes Y and A has

been programmed. Such a traversal command

G1 Y… A… produces the red, curved path for

the tool tip.

As a rule however, the behavior shown in

situation

is wanted. A straight line with

regard to the tool tip is wanted for the G1

programming even when the A axis moves

simultaneously. In this case, the machine axis

movement follows the curved path. The Z axis

also moves to hold the tool tip in a straight

line.

Important functions for 3- to 5-axis machining

3.5

Chord error

The following graphic illustrates the so-called chord error which occurs when movements that

should be defined with regard to the tool tip, are programmed for the machine axes.

The graphic on the left shows the result of the simultaneous change of the tool orientation

through movement of the A axis and the Y axis via linear interpolation of both axes. The orange

line is the programmed straight line in the Y direction. If the A axis is also moved, this results in

the green line for the movement of the tool tip. If a certain path is to be maintained for the tool tip

as in the example on the right-hand side, then position changes to the tool tip that result from

movements of the rotary axis must be compensated.

Summary of simultaneous 5-axis machining

The simultaneous 5-axis machining enables the adaptation of the tool orientation synchronously

to the linear movement in space. Without the additional control functionality of the 5-axis

transformation, this produces some unwanted side effects.

New NC programs for identical workpieces must be created for each machine type.

The NC program must be adapted for changes to the tool length.

During the programming of the machine axes, overlaid movements of the rotary and linear

axes occur which cause a linearization error for the path of the tool tip, the chord error.

Tool orientations are programmed and changed via the positions of the swivel axes. An

orientation programming and interpolation in workpiece coordinates is not possible without

suitable control functions.

Technologically, feedrates should always refer to the relative movement between the

workpiece and tool, which is not the case without 5-axis transformation. The programmed

feedrates refer to the velocity of the machine axis movements.

Normally, NC programs are created in relation to the workpiece, i.e. all the tool positions relate to

the workpiece coordinate system (WCS). In order for an NC program to be executed on the

machine, the positions must be transformed into axis movements, i.e. converted into the

machine coordinate system (MCS). The SINUMERIK is equipped with the TRAORI function to

enable this kind of transformation.

Important functions for 3- to 5-axis machining

3.5

3.5.2

The TRAORI command

The TRAORI command activates the 5-axis transformation. This enables the simultaneous 5-

axis machining without the disadvantages described in the previous section. The programming of

TRAORI changes the reference variables in the NC program. The coordinates of the X, Y, Z

linear axes now refer to the position of the tool tip.

If orientation changes are programmed in addition to the linear positions, the effects of the rotary

axis movements on the position of the tool tip are compensated by movements of the linear axes.

In addition to the explicit programming of swivel axis positions, TRAORI enables the use of

orientation information which allows also the orientation to be programmed and interpolated

independently of the kinematics.

If tools are used with a different length, the new tool data is automatically taken from the tool

table, calculated and the programmed feedrate always refers to the movement of the tool tip

relative to the workpiece.

Programming

TRAORI(n)

; Transformation On

TRAFOOF

; Transformation Off

Explanation of the commands

TRAORI

Activates the first configured orientation transformation. The

command must be programmed alone in an NC block.

TRAORI(n)

Activates the orientation transformation configured with n.

The number of the transformation (n = 1 or 2), TRAORI(1)

corresponds to TRAORI.

TRAFOON(<transformatio

If TRAORI is defined via a kinematic chain, TRAORI can also be

n name>)

activated with TRAFOON(<transformation name>).

TRAFOOF

Deactivate transformation

Depending on the configuration (depending on the machine manufacturer), TRAORI can

reset the active zero offset (e.g. G54) and the tool edge compensation (D1). Therefore it is

recommended that the zero offset and the tool edge compensation be activated again

after TRAORI is called up.

Important functions for 3- to 5-axis machining

3.5

3.5.3

Programming the tool orientation

For an active 5-axis transformation, the orientation of the tool relative to the workpiece must be

programmed in addition to the position of the tool tip. This can be performed in several ways.

Rotary axis positions (A=<value> B=<value> C=<value>)

The most common way is to program the positions of the swivel axes directly. In this way, the tool

orientations are always specified implicitly, which however are directly dependent on the

machine kinematics.

Programming rotary

The tool orientation in space is clearly defined

axes

through the specification of the rotary axis

positions for the C and A axes.

However, this also depends on the kinematics

type.

The NC program would then appear as

follows:

N020 TRAORI

…

N140 G1 A-45 C0

A commonly used machine type is shown in the graphic. However, there are also other basic

kinematics with the C and A axes as table axes or in a mixed arrangement, and in each of these

machine types different tool orientations are associated with the specified pair of C and A axis

positions. This means that the same problem exists with regard to the tool orientation as for the

linear movements. The solution there was that TRAORI enables the position of the tool tip to be

programmed independently of the machine kinematics. In the same way, kinematic-independent

options have been introduced for the tool orientation programming.

Important functions for 3- to 5-axis machining

3.5

Direction vector (A3=<value> B3=<value> C3=<value>)

The components of a vector in space are programmed during the programming of direction

vectors. Whereby A3 is associated with the X component, B3 is associated with the Y component

and C3 is associated with the Z component; the length of the vector is of no significance. For

example, A3=1 B3=1 C3=1 defines a vector with the components (1,1,1) which points in the

direction of the spatial diagonal of the coordinate system.

Programming direction

The components of the direction vector are

vector

programmed with A3, B3, and C3. The vector

points towards the tool adapter; the length of

the vector is of no significance. Vector

components that have not been programmed

are set equal to zero.

N020 TRAORI

N035 G54

N040 G1 X0 Y0 Z0 A3=1 B3=1 C3=1 F10000

The example shows the tool tip in the position

(0,0,0), and the tool shank is the diagonal of a

cube (35.26° in relation to X-Y plane).

The vectors clearly correspond to the I, J, K vectors used in CAM systems. However, as I, J, K

are reserved for the circle parameters in the CNC standard, the addresses A3, B3 and C3 are

used for the vector components in SINUMERIK.

The use of the direction vector is recommended. The accuracy level selected should be as

high as possible. As far as 5-axis programs are concerned, practical experience has

shown that good results can be achieved by using 5 decimal places for linear axes and

6 decimal places for the direction vector.

Important functions for 3- to 5-axis machining

3.5

Use of Euler or RPY angles (A2=<value> B2=<value> C2=<value>)

Instead of direct vector programming, abstract rotation angles can be used for the orientation

description. Normally, Euler angles or RPY angles (roll, pitch, yaw) are used to rotate coordinate

systems around the coordinate axes.

Euler and RPY

With Euler angles, rotation is first around the Z

axis, then around the rotated X axis and finally

around the resulting Z axis. There are different

definitions for RPY angles.

The following is used in SINUMERIK: The first

rotation is around the Z axis, the second

around the rotated Y axis and the third around

the rotated X axis.

They can also be used accordingly for the definition of a vector. This is based on a vector in the Z

direction of the coordinate system that is rotated using Euler or RPY angles. The resulting vector

is the new tool vector. The NC addresses A2, B2 and C2 are used to program the rotation

angles. The meaning of the angles, i.e. whether they are Euler angles or RPY angles, is specified

via the G codes ORIEULER and ORIRPY. This results in the following definitions:

The values programmed with A2, B2, and C2

Programming

during orientation programming are

RPY angles

interpreted as RPY angles (in degrees).

Starting from the basic position

The orientation vector is obtained by first

rotating a vector in the Z direction around the

Z axis with C2

, then rotating it around the

new Y axis with B2,

and finally rotating it

around the new X axis with A2 (Z, Y', X"). In

With C2=90°:

contrast to Euler angle programming, all three

rotated around

values here have an effect on the orientation

Z axis

vector.

With B2=45°:

Example:

rotated around

N020 TRAORI

N030 G54

N040 G0 X0 Y0 Z0

N050 C2=0 B2=0 A2=0 F10000

With A2=30°:

N060 C2=90 B2=45 A2=30

rotated around

N070 ...

X axis that is rotated

Important functions for 3- to 5-axis machining

3.5

The values programmed with A2, B2, and C2

Programming

during orientation programming are

Euler angles

interpreted as Euler angles (in degrees).

Starting from the basic position

The orientation vector is obtained by first

rotating a vector in the Z direction around the

Z axis with A2

, then rotating it around the

new X axis with B2,

and finally, rotating it

With A2=90°

around the new Z axis with C2 (Z, X', Z").

rotated

around Z axis

Example:

N020 TRAORI

N030 G54

N040 G0 X0 Y0 Z0

N050 G1 A2=0 B2=0 F1000

N060 G1 A2=90 B2=45

With B2=45°:

N070 ...

rotated around

In this case, the value of C2 (rotation around

Y axis that is

the Z axis) is meaningless and does not have

to be programmed.

Lead and tilt angles (LEAD/TILT)

In conjunction with LEAD and TILT, the orientation is programmed via a lead angle and a tilt

angle. This is the only orientation programming variant that is linked to a certain orientation

interpolation for the type of orientation definition, namely ORIPATH.

LEAD

Lead angle for programming tool orientation.

Angle relative to the surface normal vector in the plane put up by

the path tangent and the surface normal vector.

TILT

Tilt angle for programming tool orientation.

The TILT angle defines the rotation of the lead angle around the

surface normal vector

Important functions for 3- to 5-axis machining

3.5

LEAD and TILT

The resultant tool orientation is determined

from:

Path tangent

Surface normal vector

Lead angle LEAD

Tilt angle TILT at end of block

LEAD describes the angle between the sur-

face normals and the new tool orientation in

the plane set up by the path tangent and the

surface normals

The tilt angle corresponds to a rotation of the

tool in the plane perpendicular to the surface

normals

The lead angle is often used to orient the tool

at a fixed setting angle to the machining plane.

This increases the cutting performance. For

example, a ball mill touches the surface to be

machined precisely with the tool tip when the

orientation is perpendicular. However, the

rotation and therefore the cutting speed is 0 at

this point of the milling cutter.

The following program sequence corresponds

approximately to that shown in the graphic.

N10 TRAORI

N20 G1 X=0 Y0 A3=0 B3=0 C3=1

N30 ORIPATH

N40 X10 LEAD=30 TILT=10 C5=1

Important functions for 3- to 5-axis machining

3.5

As already mentioned, the lead and tilt angles are only defined in conjunction with the surface

normal vector. This is defined in the same way as the orientation vector with the components A4,

B4, C4 or A5, B5, C5: The first designate the normal vector at the start of the block, the latter at

the end of the block.

The surface normal vector is perpendicular

to the machining surface.

The start vector at the start of the block is

programmed with A4, B4, C4. The vector at

the end of the block is programmed with A5,

B5, C5.

Important functions for 3- to 5-axis machining

3.5

3.5.4

Orientation interpolation and orientation reference

In the NC program, the tool orientation relative to the workpiece is specified block-by-block by

vectors (A3, B3, C3) or angles ((axis positions A, B, C), Euler or RPY angles (A2, B2, C2) or

(LEAD/TILT)). In 5-axis simultaneous machining, these normally change in each block. If the

machine is now to be moved in accordance with the specifications of the NC program, the

orientation must be continuously changed synchronous to the path motion.

Motion interpolation in the 3-axis area

New X, Y and Z coordinates are specified block-by-block. However, there are obviously

numerous ways to move a tool from one position to the next. This can be performed along a

straight line (G1), on an arc (G2, G3) or also on a spline curve (ASPLINE, BSPLINE, CSPLINE).

In each case, there is a different movement although the programmed coordinates are identical.

Therefore, to clearly describe the desired movement, it is not sufficient to only specify the

coordinates, the way in which traversing is performed from one coordinate to the next must also

be specified. This is performed using the G codes of group 1.

Interpolation of the tool orientation in a point

In the same way, there are numerous ways to move from one tool orientation (X1, Y1, Z1) to the

next (X2, Y2, Z2). This can be performed by moving the vector in a plane, on a conical surface or

an otherwise curved surface. These are shown in the following graphics.

Important functions for 3- to 5-axis machining

3.5

Tool orientation in the 5-axis area

To change a tool orientation from the start orientation of the start block (X1, Y1, Z1) to the target

orientation of the next block (X2, Y2, Z2), it is also not sufficient to only specify the coordinates.

How the vectors move must also be defined. In a plane, on a conical surface or an otherwise

curved surface. The G codes of group 51, ORIVECT, ORIAXES, ORICONXX, ORICURVE, etc.

are used for this purpose.

This is best seen when the position of the tool tip and the tool orientation are changed

simultaneously. This can generally be described by two curves. The orange line describes the

movement of the tool tip while the green line defines the movement of a second point on the tool.

These two curves clearly describe the surface on which the tool moves. This fact is used for the

3D spline interpolation ORICURVE by displaying the orange and the green lines through spline

curves.

Important functions for 3- to 5-axis machining

3.5

Comparison of ORIVECT and ORIAXES

To illustrate the differences more clearly, let us consider the two most commonly used cases

ORIVECT and ORIAXES. As already mentioned, ORIAXES is the standard interpolation type

that is most commonly used. The rotary axes are interpolated linearly synchronous to the

movement of the tool tip. Let us consider the following situation to illustrate this type.

The following figure shows the movement of a fork head machine with C and A axes along an NC

block.

We will begin at the start of the block with position P1, the tool vector t1 and the corresponding

rotary axes positions C1 and A1. The position, the tool vector and the rotary axes positions at the

end of the block are specified with P2, t2, C2 and A2. For the interpolation of the tool tip with the

programmed velocity, the distance to the end point is divided into sections of equal size, whose

length ΔS corresponds to the interpolation cycle and the programmed feedrate. The increment is

ΔS = VT, whereby V is the velocity and T the interpolation cycle time. At constant velocity, the

entire traversing distance D between P1 and P2 is divided into nine equidistant interpolation

increments.

In the same way with ORIAXES, the difference of the rotary axis positions C2-C1 and A2 - A1 is

divided into 9 equidistant increments C and A. This means that the curve of the rotary axis

positions linearly follows the path motion.

Important functions for 3- to 5-axis machining

3.5

The circumstances are different with ORIVECT. The vector is interpolated and not the rotary

axes. For this purpose, the differential angle J between the start vector t1 and the end vector t2 is

considered. This is divided into 9 equidistant increments ΔJ in accordance with the path motion.

The intermediate vectors defined as a result are all in a plane set up by t1 and t2. A surface is

therefore defined in workpiece coordinates, in this case a plane, on which the orientation vector

moves. The possible orientation interpolations are described in the following section.

Orientation reference to the coordinate system (ORIMKS, ORIWKS)

The reference for the rotary axis interpolation is defined using the G code commands ORIMKS/

ORIWKS.

ORIMKS Tool orientation in the machine coordinate system.

With ORIMKS, the programmed orientation relates to the coordinate system defined by the

machine axes. Rotations through frames are not taken into consideration here.

ORIWKS Tool orientation in the workpiece coordinate system.

With ORIWKS, the programmed orientation relates to the workpiece coordinate system that may

be rotated in relation to the machine coordinate system using a frame.

Orientation reference

ORIMKS

The reference system for the orientation vector is the machine

coordinate system.

ORIWKS

The reference system for the orientation vector is the workpiece

(recommended)

coordinate system. Machine data is used to determine precisely

what happens.

Important functions for 3- to 5-axis machining

3.5

Orientation interpolation of the axes

Linear interpolation (ORIAXES)

Linear interpolation

The rotary axes are interpolated linearly syn-

(ORIAXES)

chronous to the path motion. In this interpola-

tion type, the orientation curve depends on the

machine kinematics. It can be used in all

cases in which it is not necessary that the tool

moves on a precisely defined surface in the

workpiece coordinate system. This is the

case, for example, in mold-making when ball

mills are used.

Axis/linear interpolation

ORIAXES

Linear interpolation of the machine axes

(recommended)

Vector interpolation (ORIVECT/ORIPLANE)

The tool vector always moves in a plane set

Vector interpolation

up by the start and end vectors. The

Large circle

interpolation type is frequently used in the

interpolation

milling of aircraft structures because the

(ORIVECT/ORIPLANE)

pockets mostly have flat and inclined walls. It

is also recommended when using toroidal

millers for face milling.

Vector interpolation

ORIVECT

Interpolation of the orientation vector in a plane (large circle

interpolation)

ORIPLANE

Interpolation in a plane (large circle interpolation), identical to

ORIVECT

Important functions for 3- to 5-axis machining

3.5

Cone surface interpolation (ORICONxx)

With cone surface interpolation, during

Cone surface

reorientation the tool moves on a

interpolation

programmable peripheral surface of a cone

(ORICONCW)

located anywhere in space.

Vector interpolation

ORICONCW

Interpolation on the peripheral surface of a cone in the clockwise

direction

Programming:

Circle end position with radius: G2 X.. Y.. Z.. CR=

End orientation vector: A3= B3= C3= or A2= B2= C2=

Vector of the cone's axis of rotation: A6= B6= C6=

Opening angle of the cone (PSI), value 0 -180 degrees:

GROOVE=

ORICONCCW

Interpolation on a peripheral surface of a cone in the

counterclockwise direction

Programming:

Circle end position with radius: G3 X.. Y.. Z.. CR=

End orientation vector: A3= B3= C3= or A2= B2= C2=

Vector of the cone's axis of rotation: A6= B6= C6=

Opening angle of the cone (PSI), value 0 -180 degrees:

GROOVE=

ORICONIO

Intermediate orientation via A7=… B7=…, C7=….

Programming:

Circle end position: CIP X.. Y.. Z..

Circle intermediate point: I1=... J2=.. K1=..

Intermediate orientation vector: A7=.. B7=.. C7=..

End orientation vector: A3= B3= C3= or A2= B2= C2=

ORICONTO

Interpolation on a peripheral surface of a cone with tangential

transition.

Programming:

Circle end position: CT X.. Y.. Z..

End orientation vector: A3= B3= C3= or A2= B2= C2=

Important functions for 3- to 5-axis machining

3.5

Spline interpolation (double spline ORICURVE)

Spline interpolation

With spline interpolation, the movement of the

Curve interpolation

orientation vector is defined by the tool tip's

(ORICURVE)

path

and the path of a second point on the

tool

If, for example, you wanted to use

circumferential milling to create an inclined

surface, you would define the surface on

which the milling cutter should move using two

spline curves at the top and bottom ends of

the tool (1, 2).

The advantage of this is that it enables you to

define a wide variety of surfaces for machining

with a high degree of precision.

Spline interpolation is the best type of

interpolation available, but it is also the most

involved and calls for special syntax in the NC

program that must be supported by the CAM

system.

Spline / double spline interpolation

ORICURVE

Orientation interpolation with specification of the tool tip motion

and that of a second point on the tool. The path of the second

point is defined via XH=… YH=… ZH=…, in conjunction with

BSPLINE as a control polygon with POLY as polynomial:

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

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

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

If the BSPLINE or POLY additional information is omitted,

straightforward linear interpolation will be performed accordingly

between the start and the end orientation.

Important functions for 3- to 5-axis machining

3.5

Path-related interpolation (ORIPATH)

Path-related

The orientation vector is set relative to the

interpolation

path and to the surface normals. The

programming is performed using the LEAD

angle and the TILT angle in conjunction with

fsfsf

the surface normal vector. LEAD describes a

rotation around the direction perpendicular to

the tangents and normals while TILT

describes a rotation of the orientation around

the surface normal vector.

The orientation interpolation with ORIPATH is

recommended when programming on the

CAM system during the machining of free-

form surfaces in tool and mold-making. The

prerequisite for this is support of the issuing of

surface normals of your CAM system.

Path-related interpolation

ORIPATH

Tool orientation in relation to the path.

This is used with the commands LEAD and TILT and the

specification of the surface normals with A4, B4, C4 and A5, B5,

C5.

Important functions for 3- to 5-axis machining

3.5

3.5.5

Example application involving TRAORI and frames

Example TOROT - Retraction from a slanted hole

When 5-axis transformation is active, TOROT generates a frame whose Z axis coincides with the

current tool orientation. This function can be used with a 5-axis program, for example, to retract

the tool after a tool breakage without collision, simply by returning the Z axis. Following tool

orientation with TOROT, all the geometry axis movements programmed will relate to the frame

generated as a result of this function.

Programming TOROT in MDI

N110

TRAORI

; Activate TRAFO

N120

TOROT

; Calculate and select return frame

N130

G1 G91 Z50 F500

; Return movement by 50 mm in Z direction in a straight

line

N140

M17

; End of subprogram

A frame containing the current tool orientation

in the Z direction is generated

This means

that in JOG mode, the tool can be returned

from the workpiece in the Z direction.

As an alternative to traversing incrementally in

MDI mode, in JOG mode you can use the

direction key to enable return in the tool

direction.

Notice:

Return is possible only in JOG mode if the

machine has been configured accordingly (Z

axis serves as the geometry axis).

TOROT to machining plane

TOROT for G17

TOROTY for G18 -> tool axis Y

TOROTX for G19 -> tool axis X

TOROT must be deselected prior to the next program start: TOROTOF.

A similar function is available in JOG with the manual retraction. After an interruption of a

tapping operation (G33/G331/G332) or a general drilling operation (tools 200 to 299) due to

power loss or a RESET at the machine control panel, you have the possibility to retract

the tool in the tool direction without damaging the tool or the workpiece.

100

Important functions for 3- to 5-axis machining

3.5

3.5.6

Useful NC commands for active TRAORI

In conjunction with the programming of TRAORI, the following NC commands can help to

simplify programming.

ORIRESET Approach basic position of the tool orientation (ORIRESET)

Through ORIRESET(.,.,.), the orientation axes of the relevant machine kinematics are traversed

linearly and synchronously from their current positions to the programmed basic positions. If a

basic position is not programmed for an axis, the position from the associated machine data

$MC_TRAFO5_ROT_AX_OFFSET_1/2 is used.

Programming:

Example of machine kinematics CA (channel axis names C, A).

ORIRESET(90, 45)

; C to 90 degrees, A to 45 degrees

ORIRESET(, 30)

; C from $MC_TRAFO5_ROT_AX_OFFSET_1/2[0], A to 30 degrees

ORIRESET( )

; C from $MC_TRAFO5_ROT_AX_OFFSET_1/2[0], A to

$MC_TRAFO5_ROT_AX_OFFSET_1/2[1]

STAT Defining the preferred direction for active TRAORI with STAT

For active TRAORI, the control automatically executes compensatory movements of the rotary

axes to achieve specific positions of the tool positioning. Because these compensatory

movements are made by the control in negative and positive rotary axis positions, the preferred

direction can be hard coded with the STAT command. The rotary axes are then moved only in

the positive or negative direction to reach the target position. For example, STAT can be used

instead of prepositioning with CYCLE800.

Programming:

STAT is programmed for ORIWKS and ORIAXES

STAT=-1; (axis remains at - position. Only for ORIAXES)

STAT=1; (axis remains at + position. Only for ORIAXES)

101

Important functions for 3- to 5-axis machining

3.6

High Speed Settings - CYCLE832

Application

You can influence the sequence of CAM programs using SINUMERIK CYCLE832. It provides

technological support for 3- and 5-axis machining in the high-speed cutting (HSC) range.

When executing CAM programs in the HSC range, the control needs to achieve high machining

feedrates. By applying different machining strategies, you can use CYCLE832 to fine-tune the

program for execution.

When roughing, the emphasis is on velocity due to the smoothing of the contour.

When finishing, the emphasis is on surface quality and accuracy.

In both cases, specifying a tolerance ensures that the correct machining contour is achieved in

order to obtain the desired surface quality and accuracy. Generally, for roughing the tolerance is

greater than for finishing.

Advanced Surface and Top Surface

For CYCLE832, as of software release V4.7 SP2, you can select between Advanced Surface

and option Top Surface.

Top Surface is an option of CYCLE832 - and is based on the COMPSURF compressor. This has

been improved for machining demanding CAD/CAM programs. The new compressor especially

compensates the potential negative impact on the surface quality for an inhomogeneous point

distribution, as is the case for inclined line-by-line finishing programs and for bidirectional milling.

The result is a uniformly perfect surface, which is essentially independent of the quality of the

CAD/CAM data.

Surface quality

Roughing

▼

Semi-finishing

▼▼

Accuracy

Velocity

Finishing

▼▼▼

Advanced Surface

Top Surface

102

Important functions for 3- to 5-axis machining

3.6

3.6.1

Parameters for CYCLE832

CYCLE832 can be set by the machine operator or, within the context of NC program generation,

by the postprocessor or programmer. Dynamic values and NC commands are adapted to

address specific user requirements and they depend on the settings of the machine data

(machine machine manufacturer).

In CYCLE832, the operator can select between the four different types of machining of the

technology group Dynamic G group 59 and activate their dynamic parameters.

CYCLE832 with Advanced Surface based on the well proven COMPCAD compressor. The new

COMPSURF compressor is used for Top Surface. Top Surface when milling inclined line-by-line

contours.

With innovated lookahead functionality, as well as harmonizing velocity profiles of adjacent paths

and optimized acceleration and jerk behavior, CYCLE832 guarantees extremely good surface

quality with short machining times.

By selecting the machining strategy, the CAM program execution is optimized for the machine.

Depending on the selected machining

the blue arrows

point in the Velocity, Surface

quality or Accuracy direction. Using the Default values softkey

preassigns the cycle

parameters, depending on the selected machining.

103

Important functions for 3- to 5-axis machining

3.6

Parameters for the High Speed Setting cycle

Advanced Surface

Top Surface

Parameterizing CYCLE832

X At Machining, select one of the deselection, finishing, semi-finishing and roughing

parameters.

X If the Top Surface option is activated, then you can select between the two motion controls.

Advanced Surface is the default setting.

X Enter a value in the Axis/contour tolerance field.

X For multi-axis programs, as of SW 4.5, you can smooth the orientation characteristic in the

cycle and apply an ORI tolerance.

X For Top Surface, smoothing can also be activated via a setting data item. When smoothing,

inhomogeneous areas along the path are smoothed.

CYCLE832 parameters (as of SW 4.7 SP2)

Machining

Finishing (_FINISH)

Selection for 3-axis programs with plain

text.

Semi-finishing (_SEMIFIN)

Choosing "Deselection" resets the values to

Roughing (_ROUGH)

the default values.

Deselection (_OFF)

Finishing (_ORI_FINISH)

Selection for multi-axis programs with

orientation tolerance in plain text.

Semi-finishing (_ORI_SEMIFIN)

Roughing (_ORI_ROUGH)

Tolerance_tol.

Chord tolerance, contour tolerance, axis

Tolerance of the linear axes

tolerance

(Chord tolerance must be imported from the CAM

system 1:1)

104

Important functions for 3- to 5-axis machining

3.6

Smoothing

Yes (_TOP_SURFACE_SMOOTH_ON)

Yes: Optimized path within the contour

(can be set via setting data item)

tolerance

Inhomogeneous areas in the path in the

No (_TOP_SURFACE_SMOOTH_OFF)

standard tolerance range of 10 µm are

reliably smoothed. The workpiece assumes

a shiny surface.

No: Close-contour path

The specified contour is precisely followed.

Engraving and geometries with a depth <=

0.005 mm = 5 µm are visible on the

workpiece surface.

Multi-axis

No: For 3-axis programs without rotary

program

(can be set via setting data item)

axes. The value 1 is entered automatically

Yes

Yes: For multi-axis programs with rotary

axes. The orientation smoothing is

activated; ORI tolerance > 0° must be

entered.

ORI tolerance

OTOL tolerance

Has two meanings:

Smoothing tolerance of the rotary axes

(approx. factor 10 of the linear tolerance)

for 5-axis transformation TRAORI

Orientation tolerance for the smoothing

of vectors with active ORISON

CYCLE832 is based on the use of G1 blocks, also G0, G2 and G3, depending on the

machine setting.

When using the ORI tolerance, only for Advance Surface, after calling CYCLE832 does

orientation smoothing activation have to be programmed using ORISON. You should not

program ORISON for 5-axis hobbing/circumferential milling as this can result in contour

errors. ORISON is deactivated automatically for Top Surface (COMPSURF).

CYCLE832 structure

CAM systems frequently specify via the postprocessor that CYCLE832 is output directly in the

geometry program. Therefore, make sure that CYCLE832 is programmed in the geometry

program for your start program. CYCLE832 is then automatically selected and deselected in the

subprogram. The start program then only contains the calls of the subprograms with the

geometry data.

This means that you can apply the cycle to the complete geometry or - depending on the

transparency of the CAM program - to individual program sections or free-form surfaces.

Program CYCLE832 after the tool change. After calling CYCLE832, only the geometry data

should still be programmed.

105

Important functions for 3- to 5-axis machining

3.6

CYCLE832(tolerance, technology, ORI tolerance)

Programming the cycle:

Tolerance (chord tolerance)

Technology

0 = Deselection

1 = Finishing (_FINISH)▼▼▼

2 = Semi-finishing (_SEMIFIN)▼▼

3 = Roughing (_ROUGH)▼

11 = Finishing multi-axis program (_ORI_FINISH)▼▼▼

12 = Semi-finishing multi-axis program (_ORI_SEMIFIN)▼▼

13 = Roughing multi-axis program (_ORI_ROUGH)▼

1000000 = Top Surface without smoothing

2000000 = Top Surface with smoothing

ORI tolerance

Orientation tolerance or version identifier CYCLE832. Is required

when executing an HSC program on machines with dynamic

orientation transformation (e.g. 5-axis machining). Parameter

S_OTOL must be programmed. This also applies for applications

on 3-axis machines for programs without orientation of the tool

(S_OTOL = 1).

CYCLE832(0.05,12,0.5)

CYCLE832 for semi-finishing with tolerance 0.05 with orientation

smoothing and ORI tolerance 0.5.

CYCLE832(0.01,_TOP_SURFACE_SMOOTH_OFF+_ORI_FINISH,0.1)

CYCLE832 for finishing with 0.01 tolerance, Top Surface activated,

smoothing off and orientation smoothing with ORI tolerance 0.1

CYCLE832 Advanced Surface programming example

N10

T1 D1

; Tool selection

N20

G54

; Select tool zero

N30

M3 S1200

; Clockwise spindle rotation and speed

N40

CYCLE832(0.1,3,1)

; 3-axis program, tolerance value 0.1

N50

; [3] = Roughing, [1] = Standard without ORI

N60

EXTCALL "CAM_ROUGH_0"

; Call subprogram CAM_ROUGH_0

N65

CYCLE832(0,_OFF,1)

; Deselection CYCLE832

N70

CYCLE832(0.1,_ROUGH,1)

; 3-axis program, tolerance value 0.1

N80

; [_ROUGH] = Roughing as plain text, [1] = Standard without ORI

N90

EXTCALL "CAM_ROUGH_1"

; Call subprogram CAM_ROUGH_1

N95

CYCLE832(0,_OFF,1)

; Deselection CYCLE832

N100

CYCLE832(0.01,11,0.1)

; 5-axis program (with orientation), tolerance value 0.01

N110

; [11] = finishing, [0.1]= ORI tolerance 0.1

N120

ORISON

; Activation of the orientation smoothing

N130

EXTCALL "CAM_FINISH_0"

; call subprogram CAM_FINISH_0

N135

CYCLE832(0,_OFF,1)

; Deselection CYCLE832

N140

CYCLE832(0.005,_ORI_FINISH,0.05)

; 5-axis program (with orientation), tolerance value 0.005

N150

; [_ORI_FINISH] = finishing as plain text, [0.05]= ORI tolerance 0.05

N160

ORISON

; Activation of the orientation smoothing

N170

EXTCALL "CAM_FINISH_1"

; call subprogram CAM_FINISH_1

N180

CYCLE832(0,_OFF,1)

; Deselection CYCLE832

N200

M30

; End of program

106

Important functions for 3- to 5-axis machining

3.6

CYCLE832 Top Surface programming example

N10

T1 D1

; Tool selection

N20

G54

; Select tool zero

N30

M3 S1200

; Clockwise spindle rotation and speed

N40

CYCLE832(0.1,_TOP_SURFACE_SMOOTH_OFF+_ROUGH,1)

N50

; 3-axis program, tolerance value 0.1, [_TOP_SURFACE_SMOOTH_OFF] = Top Surface active, smoothing off

N55

; [_ROUGH] = roughing, [1] = standard without ORI

N60

EXTCALL "CAM_ROUGH_0"

; Call subprogram CAM_ROUGH_0

N65

CYCLE832(0,_OFF,1)

; Deselection CYCLE832

N70

CYCLE832(0.05,_TOP_SURFACE_SMOOTH_OFF+_SEMIFIN,1)

N80

; 3-axis program, tolerance value 0.05, [_TOP_SURFACE_SMOOTH_OFF] = Top Surface active, smoothing off

N85

; [_SEMIFIN] = semi-finishing, [1] = standard without ORI

N90

EXTCALL "CAM_SEMIF_1"

; Call subprogram CAM_SEMIF_1

N95

CYCLE832(0,_OFF,1)

; Deselection CYCLE832

N100

CYCLE832(0.001,_TOP_SURFACE_SMOOTH_ON+_ORI_FINISH,0.01)

N110

; 5-axis program, tolerance value 0.001, [_TOP_SURFACE_SMOOTH_ON] = Top Surface active, smoothing on

N120

; [_ORI_FINISH] = 5-axis finishing as plain text, [0.01]= ORI tolerance 0.01

N130

EXTCALL "CAM_FINISH_0"

; Call subprogram CAM_FINISH_0

N135

CYCLE832(0,_OFF,1)

; Deselection CYCLE832

N200

M30

; End of program

Before the functions listed here can be used, the machine manufacturer must have

optimized the CNC machine correctly.

107

Important functions for 3- to 5-axis machining

3.6

CYLCE832 in older software releases

Because of the continuous further development of CYCLE832, the syntax and also the functional

scope of the cycle differs between the software releases. Therefore, note the new syntax of

CYCLE832 when using older programs. A compatibility mode can be set via a machine data

item. Contact the machine manufacturer if you have any questions on compatibility.

Software release

NC code

SINUMERIK up to SW 7.5

CYCLE832(tolerance, technology)

CYCLE832(0.01,112101)

SINUMERIK Operate SW 2.6

CYCLE832(tolerance, machining, version ID)

CYCLE832(0.1,3,1)

SINUMERIK Operate

CYCLE832(tolerance, machining, version ID) and ORISON

SW 2.7 to SW 4.4

can be programmed separately

CYCLE832(0.005,1,1)

ORISON

OTOL=0.05

When using the ORI tolerance, the activation of the orientation

smoothing with ORISON must be explicitly programmed after

the call of CYCLE832.

SINUMERIK Operate

CYCLE832(tolerance, machining, ORI tolerance) and

SW 4.5

ORISON can be separately programmed

CYCLE832(0.005,_ORI_FINISH,0.5)

ORISON

When using the ORI tolerance in the CYCLE832, depending

on the configuration of CUST_832, after calling CYCLE832,

the activation of orientation smoothing must be programmed

with ORISON.

108

Important functions for 3- to 5-axis machining

3.6

3.6.2

CYCLE832 and CUST_832

The manufacturer cycle CUST_832 is available for individual adaptation of CYCLE832. This is

individually adapted according to the machine by the machine manufacturer. Special NC

commands for machining are also set in CUST_832. As a consequence, the parameters in the

CYCLE832 dialog can deviate from the descriptions in Section 3.6.1 if the machine manufacturer

has made specific adaptations.

NC commands in connection with Advanced Surface and Top Surface

The following NC code commands are preset in CUST_832.SPF and are activated when the

technology groups are selected in CYCLE832:

DYNNORM, DYNROUGH, DYNSEMIFIN, DYNFINISH (G code group 59).

COMPCAD makes it possible to combine part programs with short linear blocks (G1), with

the associated tolerance, using polynomials.

COMPSURF, compressor ensures a better workpiece surface for inclined line-by-line

finishing programs, poor data quality - or for example, irregular point distribution in NC

programs from the CAD/CAM system.

SOFT (G code group 21) activates the jerk-limited velocity control.

G645 (G code group 10) switches to the continuous-path mode (Look Ahead).

FIFOCTRL (G code group 4) switches to the automatic pre-processing memory control.

FFWON (G code group 24) switches to the parameterized feedforward control (speed or

acceleration feedforward control). Can be optionally activated in CUST_832.

Important NC commands for 5-axis machining

In CUST_832.SPF, the following NC code commands can be preset by the machine

manufacturer.

TRAORI activates the 5-axis transformation set in the transformer machine data and must be

programmed alone in the block.

UPATH (G code group 45) ensures synchronous movements of the rotary and linear axes in

5-axis spline interpolation, as performed with active compressor, for example.

ORIAXES (G code group 51) linearly interpolates the orientation axes in the block up to the

end of block.

ORIWKS (G code group 25) defines the workpiece coordinate system for orientation

programming.

ORISON (G code group 61) activates the orientation smoothing for 5-axis machining with

active 5-axis transformation (TRAORI).

You can see which functions of CYCLE832 are currently active during processing in the

"All G functions" display.See "Executing programs (AUTOMATIC)" on page 64.

In the following sections, you will find the relevant machine functions such as Compressor and

Look Ahead, which are only explained briefly here, because they are automatically called up with

optimal values by CYCLE832 or CUST_832.

109

Important functions for 3- to 5-axis machining

3.7

Advanced Surface and Top Surface

SINUMERIK bundles a range of special mold-making functions under Advanced Surface and

Top Surface. This intelligent motion control achieves optimum workpiece surfaces while at the

same time providing maximum machining velocity. Advanced Surface or Top Surface are

activated automatically when you work with CYCLE832.

When the new motion control is used, an optimized Look Ahead function contributes to perfect

surface quality through reproducible results in adjacent milling paths, accuracy and increased

velocity. The compressor ensures precise contour accuracy and maximum machining velocity.

Intelligent jerk limitation reduces the stress on the machines mechanical system and allows soft

acceleration and braking of the axes, therefore extending the machine service life.

One important advance is the automatic harmonization of the velocity profiles on adjacent milling

paths by means of CNC. It also works for the forward/backward line-by-line milling of contours

and free-form surfaces and it directly leads to increased surface quality.

Top Surface is based on the COMPSURF compressor. This has been improved for machining

demanding CAD/CAM programs.

Without

With

Advanced Surface

Top Surface

Increased machining velocity due to an

improved velocity profile. The red areas show

the maximum velocity.

Perfect surface quality thanks to reproducible

results in adjacent milling paths. The surface

is much more homogeneous.

The compressor does not only work via G1

blocks. It also compresses rapid traverse

movements G0 using smoothing. The velocity

remains at a constant high level during the

entire machining process (red areas).

110

Important functions for 3- to 5-axis machining

3.7

Without

With

Top Surface

Significantly better workpiece surfaces for

bidirectional milling using direction-

independent identical smoothing of the milling

paths - and essentially independent of the

CAM data quality.

Top Surface

smoothing on

smoothing off

When smoothing is active, unevenness in the

micrometer range is smoothed within the

tolerance.

If smoothing is set to "no", then the specified

contour is precisely machined.

Advanced Surface validation / Top Surface machine data

A check program is available to validate the correctly set machine data. This program provides

support to set the machine data for Advanced Surface and Top Surface as recommended. It

checks the machine data and writes an overview of the machine data with details of the values

that differ from the recommended values.

The check program and the associated documentation can be downloaded from the

Industry Online Support Portal.

>> https://support.industry.siemens.com/cs/ww/en/view/109738423

111

Important functions for 3- to 5-axis machining

3.7

3.7.1

Compressor (COMPCAD, COMPSURF)

The compressor is called in CYCLE832. If it is to be programmed separately, then proceed as

described below. The common objective of compressor functions is to optimize the surface

quality and machining velocity by achieving continuous block transitions and increasing the path

length for each block. You can use machine data to set whether only G1 blocks or G2/G3 or G0

blocks should also be compressed.

Explanation of the commands

COMPOF

Compressor off

COMPCAD

Compressor on - surface quality and velocity are further

(default for

optimized.

Advanced Surface)

COMPCAD smooths the points along the characteristic before

approximation

(B spline) and offers, at a high path velocity, the highest degree of

accuracy with transitions that have a constant acceleration rate.

Preferably used to mill free-form surfaces (recommended).

COMPCURV

Compressor on.

(do not use anymore)

Blocks are approached using a polynomial. Block transitions are

jerk-free. Preferably used for circumferential milling.

COMPSURF

Compressor on.

(default for

The COMPSURF compressor ensures a significantly improved

Top Surface)

workpiece surface for inclined line-by-line finishing programs,

poor data quality - or for example, irregular point distribution in NC

programs from the CAD/CAM system. Further, COMPSURF

improves complying with acceleration and jerk limits. As a

consequence, machine-specific dynamic parameters can be

increased.

Operating principle of the compressor

In accordance with the specified tolerance

band, the compressor

takes a sequence

of motion commands

combines them and

compresses them into a spline

, which can

be directly executed by the control. A new

contour is created whose characteristic lies

within the specified tolerance range.

The compressor generates smooth paths and

paths with constant curvature. The constant

curvature results in a steady velocity and

acceleration characteristic, meaning that the

machine can run at higher velocities, thereby

increasing productivity.

112

Important functions for 3- to 5-axis machining

3.7

3.7.2

Continuous-path mode, Look Ahead - G64, G645

In continuous-path mode, the path velocity at the end of the block (for the block change) is not

decelerated to a level which would permit the fulfillment of an exact stop criterion. The objective

of this mode is, in fact, to avoid rapid deceleration of the path axes at the block-change point so

that the axis velocity remains as constant as possible when the program moves to the next block.

To achieve this objective, the Look Ahead function is also activated when the continuous-path

mode is selected.

Explanation of the commands

G64

Continuous-path mode - Look Ahead where the axis only brakes

at corners

G645

Continuous-path mode with corner smoothing and tangential

(recommended)

block transitions within the defined tolerances.

With G645, the smoothing movement is defined so that the

acceleration of all axes involved remains smooth (no jumps) and

the parameterized maximum deviations from the original contour

are not exceeded.

In connection with Advanced Surface, it is recommended that

you only work with G645.

Application of G64, G645

The objective of continuous-path mode is to

increase the velocity and harmonize the

traversing behavior. This is implemented by

two functions.

Look Ahead - anticipatory velocity control

The control calculates several NC blocks in

advance and determines a modal velocity

profile. The way in which this velocity control is

calculated can be set using the functions G64,

etc.

Corner rounding

The Look Ahead function also means that the

control is able to smooth the corners that it

identifies. This means that the programmed

corner points are, therefore, not approached

exactly. Sharp corners can be rounded.

These two functions mean that the contour is

created with a uniform path velocity profile.

This results in improved cutting conditions,

increases the surface quality and reduces the

machining time.

113

Important functions for 3- to 5-axis machining

3.7

To round sharp corners,

for example, the

continuous-path command G645 forms

transition elements

at the block

boundaries. The continuous-path commands

differ in terms of how they form these

transition elements.

With G645, rounding blocks are also

generated on tangential block transitions if the

curvature of the original contour exhibits a

jump in at least one axis.

We recommend G645 for free-form surface applications.

114

Important functions for 3- to 5-axis machining

3.7

3.7.3

Feedforward control and jerk limitation - FFWON,

SOFT, ...

Feedforward control and jerk limitation are called in CUST_832 on a combined basis. This is

because this combination offers ideal conditions for free-form surface milling. These functions

are set by the machine manufacturer.

Explanation of the commands

FFWON

Feedforward control "on"

(recommended)

FFWOF

Feedforward control "off"

BRISK

Without jerk limitation

(not recommended)

Path axes accelerate abruptly

SOFT

With jerk limitation

(recommended)

Jerk-limited acceleration of the path axes

Axial jerk limitation

Jerk limitation function

To make acceleration as smooth on the

Velocity profile

machine as possible, the acceleration profile

of the axes can be influenced using the

commands Soft and Brisk. If Soft is

BRISK

SOFT

activated, the acceleration behavior does not

change abruptly but is increased in the form of

a linear characteristic. This helps to protect the

machine and improves the surface quality of

workpieces, as much less machine resonance

time-optimized

spares the mechanical parts

is generated.

BRISK:

Acceleration behavior: Path axes accelerate

abruptly in accordance with the set machine

Acceleration profile

data.

The axis slides accelerate at the maximum

rate until the feedrate is achieved. BRISK

enables time-optimized machining, but with

jumps in the acceleration curve..

SOFT:

Acceleration behavior: Jerk-limited

acceleration of the path axes.

The axis slides accelerate at a constant rate

until the feedrate is achieved. As a result of

the jerk-free acceleration characteristic, SOFT

permits a higher path accuracy and less stress

on the machine.

115

Important functions for 3- to 5-axis machining

3.7

Feedforward control.

In cases where axes are not feedforward-con-

trolled, the following error results in a contour

error whose severity is determined by the

velocity

. Generally, this will manifest itself

in the form of a narrowing of the radius

curved contours. The following error depends

on the servo gain factor that is set (dependent

on mechanics) and the axis velocity.

The FFWON feedforward control function

brings the velocity-dependent following error

down toward zero during path traversal. Tra-

versing with feedforward control permits

higher path accuracy and thus improved

machining results.

3.7.4

Smoothing tolerance CTOL, OTOL, ATOL

The tolerance for linear and rotary axes for smoothing was previously set with CYCLE832. As of

SW 2.7 this is implemented via the functions CTOL (contour tolerance), OTOL (orientation

tolerance), and ATOL (axis-specific tolerance).

The CTOL, OTOL, and ATOL commands can be used to adapt the machining tolerances defined

for the compressor functions (COMPCAD), the smoothing types G645, and the orientation

ORISON using machine and setting data in the NC program.

The tolerance value for CTOL is set by CYCLE832. OTOL is calculated in the cycle. Since OTOL

also has an effect on ORISON by default, it is important when activating ORISON in the cycle (or

manually) to ensure that the orientation tolerance is not too great, because otherwise too much

orientation smoothing will result. In most cases, over-smoothing occurs during roughing

operations.

3.7.5

Path reference UPATH/SPATH

During polynomial interpolation, there may be a requirement for two different relationships

between the velocity-determining FGROUP axes and the other path axes. The path axes that are

not included in the FGROUP should either be routed synchronously to the path of the FGROUP

axes or to the curve parameters. Therefore, for the axes that are not contained in FGROUP,

there are two ways to follow the path:

SPATH synchronous to path S

UPATH synchronous to the curve parameter

Both types of path interpolation are needed for different applications and can be changed over

via G codes SPATH and UPATH.

UPATH is recommended for programming with active 5-axis transformation (TRAORI) and

is preset in the manufacturer cycle CUST_832.

116

Important functions for 3- to 5-axis machining

3.7

3.7.6

Smoothing the orientation characteristic (ORISON,

ORISOF)

The ORISON function can be used to smooth fluctuating orientation across several blocks. The

aim is to achieve a smooth characteristic for the orientation and therefore a more harmonious

movement of the axes.

For 5-axis programs generated by CAD/CAM systems in which the milling paths and direction

vectors are specified for the tool, the programs often contain inharmonic changes of the tool

orientation which cause sudden movements of the rotary axes and therefore, because of the

compensatory movements, also of the linear axes. Even if these deviations are only minimal,

they will lead to compensatory movements in the linear axes, which will manifest themselves in

slowed movements or even stopping in the path. The consequences are visible traces on the

workpiece surface and longer machining time.

With ORISON, the orientation is smoothed irrespective of the contour because the movement of

the rotary axes and the linear axes is much more harmonious. This results in higher machining

velocities and shorter machining times.

Up to SW 4.5, ORISON orientation smoothing is not part of CYCLE832 and it must therefore be

programmed separately with the desired vector smoothing in the NC program in the case of a 5-

axis program with orientation interpolation. If the ORISON function is to be activated

automatically with active 5-axis transformation, then this setting can be made in CUST_832 by

the OEM. Depending on the orientation tolerance, the NC command ORISON is activated in the

manufacturer cycle CUST_832 and is then also available as multi-axis program parameter

with ORI tolerance in CYCLE832.

ORISOF smoothing off

ORISON smoothing on

ORISON is deactivated automatically when using Top Surface (COMPSURF). Therefore,

after CYCLE832 with Top Surface do not program ORISON.

117

Important functions for 3- to 5-axis machining

3.7

ORISON programming (without CYCLE832)

N110

TRAORI

; Activation of orientation transformation.

N120

CYCLE832(0.005,1,1)

N130

ORISON

; Activation of orientation smoothing

N140

OTOL=0.5

; Specify tolerance

N150

G1 X10 A3=1 B3=0 C3=1

; Geometry program

N990

ORISOF

; Deactivation of orientation smoothing

ORISON programming (with CYCLE832)

N110

TRAORI

; Activation of orientation transformation.

N120

CYCLE832(0.005,_ORI_FINISH,0.5)

N130

ORISON

; Activation of the orientation smoothing

N140

G1 X10 A3=1 B3=0 C3=1

; Geometry program

N990

M30

; End of program

3.7.7

Technology G groups

Using the "Technology" G group, the appropriate dynamic response can be activated on the

machine for 5 varying technological machining operations. The dynamic values and G codes are

configured and set by the machine manufacturer.

Five dynamic response settings are available in the Technology G code group:

DYNORM for standard dynamic response

DYNPOS for positioning mode, tapping

DYNROUGH for roughing

DYNSEMIFIN for semi-finishing

DYNFINISH for finishing

The G groups are switched and activated automatically when the machining method (e.g.

finishing or roughing with CYCLE832 or CUST_832) is selected.

Dynamic parameters can be adapted to the respective machining operation with the technology

G groups. Using the commands of technology G group 59, the value of channel and axis-specific

machine data is activated using the corresponding array index. These are, for example, jerk and

acceleration values.

118

Important functions for 3- to 5-axis machining

3.7

3.7.8

Pre-processing memory control FIFOCTRL

Mold-making programs are generally executed directly from the hard drive or an external storage

medium (e.g. USB flash drive, CF card). The maximum number of NC blocks that are loaded in

the NC memory can be set via machine data.

During processing of these NC programs, the interpolation memory may run out. In this case, the

NC will stop until data is reloaded. To counter this, the pre-processing memory control

FIFOCTRL is used. For very small distances between points in a mold-making program, it is

necessary to keep the fill level as high as possible in order prevent dropping to 0% (interpolation

dip).

The pre-processing memory control FIFOCTRL is automatically called up by CYCLE832 or

CUST_832. It is deselected with STARTFIFO.

You can open the fill level of the interpolation buffer as follows:

X In the Diagnostics menu > select the System utilization softkey.

119

Important functions for 3- to 5-axis machining

3.8

Milling radius compensation 2D/3D-WRK

In the following, we will consider the expansion of the conventional 2-dimensional cutter radius

compensation to three dimensions. Normally the compensation is activated by the G codes G41/

G42 (left or right) and deactivated by G40. After activation, the control calculates an offset curve

with an offset the size of the cutter radius.

2-dimensional cutter

Center-point path

radius compensation

cutter

Contour

G41/G450

G41/G451

3.8.1

3D-WRK cutter radius compensation for

circumferential and face milling

The 3-dimensional case is more complicated. In two dimensions, it is implicitly clear that the tool

(standard tool) is aligned perpendicular to the compensation plane and therefore the

compensated path is always perpendicular to the path tangent in the X-Y plane. In three

dimensions, the tool orientation normally changes continuously and therefore the compensation

direction must also change. It is now defined by a vector in space. We must distinguish between

two situations. On the one hand, the circumferential milling for structural parts, and on the other

hand, the face milling for free-form surfaces that only requires a constant compensation value for

the Z axis in the 2-dimensional case.

CUT3DC/CUT3DCD circumferential milling

CUT3DF/CUT3DFD face milling

3-dimensional cutter

Green: Direction of compensation

radius compensation

Because in practice, suitable standard tools are often not available, a tool that does not deviate

too much from a standard tool (up to 10%) can be used.

120

Important functions for 3- to 5-axis machining

3.8

3.8.2

CUT3DC/CUT3DCD circumferential milling

In circumferential milling, the direction of compensation is always perpendicular to the plane on

which the cutter is moving. This is always defined by the current path tangent and the tool vector

and normally changes in each interpolation increment. It is defined with CUT3DC/CUT3DCD and

activated with G41/G42 (left/right).

The properties of the compensations for circumferential milling are compared in the table.

CUT3DC

CUT3DCD

(SINUMERIK 840D sl and powerline)

(SINUMERIK 840D sl as of V4.7 SP3 HF1)

Calculation of the tool compensation in the

Calculation of the tool compensation /

control/CNC

standard tool in CAD/CAM and calculation

of the difference by entering the wear in the

control/CNC.

Supplementary conditions

Can be used only to a limited extent

Can be used with compressor:

COMPCAD - Advanced Surface

Can be used only to a limited extent with

COMPSURF - Top Surface

compressor:

COMPCAD - Advanced Surface

The tools should have maximum 5-10%

COMPSURF - Top Surface

negative wear of the standard tool.

We recommend the use of the CUT3DCD function for circumferential milling.

Programming circumferential milling with CUT3DCD

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

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

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

When calculating the 3D tool radius compensation, only the wear value of the radius of the

active tool ($TC_DP15,$TC_DP16) and any programmed tool compensation offsets OFFN

and TOFFR/TOFFL are taken into account. The basic radius ($TC_DP6) of the active tool is

not taken into account. Additional information, basic length = $TC_DP3.

CUT3DCD can be used with various types of tool orientation (TRAORI active!)

Direction vector

CUT3DCD G41 G01 X145.983 Y99.000 Z-20.876 A3=0.5 B3=0 C3=1

Round axis values

CUT3DCD G41 G01 X145.983 Y99.000 Z-20.876 B-26.56 C0

The CUT3DCD 3D radius compensation is restricted to cylindrical tools.

121

Important functions for 3- to 5-axis machining

3.8

CUT3DCD programming Finishing NC program, 5-axis program

example

N1 G17 G40 G90

N2 CYCLE800()

N3 TRAFOOF

N4 T="CUTTER_10"

N5 M6

N6 S15061 M3

N7 CYCLE800(0,"TISCH",100000,27,0,0,0,288.079,0,-10.196,0,0,0,-1,0,1)

N8 G00 X-13.532 Y-24.856 M03

N9 TRAORI

N10 ORIWKS ORIAXES

N11 G54

N12 TOFFL=0

N13 TOFFR=0

N14 CYCLE800()

N15 CYCLE832(0.05,_TOP_SURFACE_SMOOTH_ON+_ORI_SEMIFIN,0.1)

N16 G0 X0 Y0 Z100.0

N17 CUT3DCD

N18 G41

N19 G1 X-5.945 Y-60.546 A3=0.021144 B3=0.341366 C3=0.939693 F2500

N20 Z5.502 A3=0.021144 B3=0.341366 C3=0.939693

N21 G1 Z0.502 A3=0.021144 B3=0.341366 C3=0.939693 F2500

N22 G1 X-5.743 Y-59.698 A3=0.021144 B3=0.341366 C3=0.939693 F500

……

N17525 g40 X0 Y0

N17526 CYCLE832(0,_OFF,1)

N17528 TRAFOOF

N17529 M17

3.8.3

CUT3DF/CUT3DFD face milling

The situation is also more complicated with face milling. Since the tool is not always

perpendicular to the plane to be machined as with two dimensions, a constant offset is no longer

sufficient. The compensation value and the compensation direction now depend on the tool

radius, the rounding radius and of course on the tool orientation relative to the workpiece surface.

This means that we require additional information about the surface. This is defined by

programming the normal vectors A4, B4, C4 (start of block) and A5, B5, C5 (end of block -

recommended programming).

The compensation is defined with CUT3DF/CUT3DFD and activated with G41/G42, whereby

there is no difference between G41 and G42 in this case.

The activation must be performed in a linear block (G0/G1). Switching off with G40 can be made

in a linear block or in a separate NC block. A change of the 3D TRC variant with active tool radius

compensation is ignored without alarm.

Before switching on CUT3DFD with G41/G42, Top Surface / COMPSURF / CYCLE832 must be

activated, not immediately before tooling, but rather approximately 1000 x CTOL = path before

the tooling or G41/G42 programmed, e.g. 1000 x 0.01 mm = 10 mm.

For traversing motions in the orientation direction of the tool, alarm 10769 is triggered and

machining stopped. As workaround, a G40 and then a G41/G42 can be programmed again for

the machining.

122

Important functions for 3- to 5-axis machining

3.8

The properties of the compensations for face milling are compared in the table.

CUT3DF

CUT3DFD

(SINUMERIK 840D sl and powerline)

(SINUMERIK 840D sl as of V4.8 SP2)

Calculation of the tool compensation in the

Calculation of the tool compensation /

control/CNC

standard tool in CAD/CAM and calculation

of the difference by entering the wear in the

control/CNC.

Supplementary conditions

Can be used with G64/G642/G645

Can be used only with compressor:

COMPSURF - Top Surface

Can be used only to a limited extent with

compressor:

The tools should have maximum 5-10%

COMPCAD - Advanced Surface

negative wear of the standard tool.

COMPSURF - Top Surface

We recommend the use of the CUT3DFD function for face milling.

Programming face milling with CUT3DFD

CUT3DFD can be used without additional tool orientation as 3-axis program, purely based

on the surface normal vector.

CUT3DFD G41 G01 X145.983 Y99.000 Z-20.876 A5=0.643 B5=0 C5=0.357

CUT3DFD can be used as 5-axis program with various types of tool orientation (TRAORI

active!)

Direction vector

CUT3DFD G41 G01 X145.983 Y99.000 Z-20.876 A3=0.5 B3=0 C3=1 A5=0.643 B5=0

C5=0.357

Round axis values

CUT3DFD G41 G01 X145.983 Y99.000 Z-20.876 B-26.56 C0 A5=0.643 B5=0 C5=0.357

The CUT3DFD 3D radius compensation acts for all tool types for machining free-form

surfaces.

123

Important functions for 3- to 5-axis machining

3.8

Face milling with perpendicular tool orientation

Face milling with any tool orientation

'LUHFWLRQ YHFWRU RU URWDU\

D[LV GLUHFWO\ RI WKH WRRO LQ

WKH &1& EORFN

1RUPHG WRRO IRU WKH

&$0 RXSXW

&$0 RXWSXW

6XUIDFH QRUPDO YHFWRU LQ

WKH FRQWDFW SRLQW LQ WKH

6XUIDFH QRUPDO YHFWRU LQ

&1& EORFN

3URJUDPPHG

1& &RGH LQ WKH

WKH FRQWDFW SRLQW LQ WKH

1& &RGH LQ

SDUWSURJUDPP

&1& EORFN

SDUWSURJUDPP

&87 ')' )DFH PLOOLQJ LQ YHUWLFDO WRRO RULHQWDWLRQ

&87 ')' )DFH PLOOLQJ LQ DQ\ RULHQWDWLRQ

CUT3DFD programming Finishing NC program, 3-axis program

example

N1 G17 G40 G90

N2 T="BALL_D16" D1

N3 M6

N4 S15061 M3

N5 G54

N6 TOFFL=0

N7 TOFFR=0

N8 CYCLE832(0.01,_TOP_SURFACE_SMOOTH_ON+_FINISH,1)

N9 R2=5000

N10 R3=5000

N11 R4=35000

N12 G0 X-11.0000 Y0.0000 Z74.0000

N13 M3

N14 G0 X-11.0000 Y0.0000 Z-26.0000

N15 G41 CUT3DFD

N16 G1 X-10.2235 Z-25.8978 A5=0.0000000 B5=0.0000000 C5=1.0000000 F=R2

N17 G1 X-9.5000 Z-25.5981 A5=0.0000000 B5=0.0000000 C5=1.0000000

N18 G1 X-8.8787 Z-25.1213 A5=0.0000000 B5=0.0000000 C5=1.0000000

N19 G1 X-8.4019 Z-24.5000 A5=0.0000000 B5=0.0000000 C5=1.0000000

N20 G1 X-8.1022 Z-23.7765 A5=0.0000000 B5=0.0000000 C5=1.0000000

N21 G1 X-8.0000 Z-23.0000 A5=-1.0000000 B5=0.0000000 C5=0.0000000

N22 G1 X-8.0000 Z-18.0000 A5=-1.0000000 B5=0.0000000 C5=0.0000000 F=R3

N23 G1 X-7.9904 Z-17.6075 A5=-0.9987955 B5=0.0000000 C5=0.0490677

N38 G01 G40 X-20.168 Y7.651 Z23.355

N39 G01 X-17.453 Y8.537 Z39.237

N40 G00 X-14.929 Y9.361 Z54.001

N41 CYCLE832(0,_OFF,1)

N42 TRAFOOF

N43 M30

124

Important functions for 3- to 5-axis machining

3.8

CUT3DFD programming Finishing NC program, 5-axis program

example

N1 G17 G40 G90

N2 CYCLE800()

N3 TRAFOOF

N4 T="BALL_D6" D1

N5 M6

N6 S15061 M3

N7 CYCLE800(0,"TABLE",100000,27,0,0,0,288.079,0,-10.196,0,0,0,-1,0,1)

N8 G00 X-13.532 Y-24.856 M03

N9 TRAORI

N10 ORIWKS ORIAXES

N11 G54

N12 TOFFL=0

N13 TOFFR=0

N14 CYCLE800()

N15 CYCLE832(0.05,_TOP_SURFACE_SMOOTH_ON+_ORI_SEMIFIN,1)

N16 G00 X-18.974 Y8.041 Z54.001 A-10.196 C=DC(+288.079)

N17 G00 X-19.647 Y7.821 Z50.064 A-10.196 C=DC(+288.079)

N18 G01 X-20.168 Y7.651 Z47.016 F1485.4

N19 G41 CUT3DFD

N20 G01 X-20.505 Y7.541 Z45.047 A3=+.168277208 B3=+.054933772 C3=+.984207835

A5=+1. B5=-.000003008 C5=+.000000718

N21 G01 X-20.506 Y7.365 Z45.047 A3=+.168631651 B3=+.053835903 C3=+.984207835

A5=+1. B5=+.000004199 C5=+.000000719

N22 G01 X-20.507 Y7.194 Z45.047 A3=+.168973327 B3=+.052753699 C3=+.984207835

A5=+1. B5=-.000007571 C5=+.000000721

N23 G01 X-20.508 Y7.025 Z45.047 A3=+.169308954 B3=+.051666392 C3=+.984207835

A5=+1. B5=-.000002005 C5=+.000000722

N38 G01 G40 X-20.168 Y7.651 Z23.355

N39 G01 X-17.453 Y8.537 Z39.237

N40 G00 X-14.929 Y9.361 Z54.001

N41 CYCLE832(0,_OFF,1)

N42 TRAFOOF

N43 M30

125

Important functions for 3- to 5-axis machining

3.8

3.8.4

Circumferential milling with limiting surfaces

(CUT3DCC/CUT3DCCD)

A combination of these two methods is used when machining special structural components in

the aviation industry. Pockets are machined where the wall inclination forms an acute angle to

the floor. The wall is machined with 5-axis circumferential milling with simultaneous contact with

the floor. If a large cutter is used in this situation, compensation must be performed

simultaneously perpendicular to the wall and along the cutter axis in order to avoid contour

violations of the floor.

Circumferential milling

Standard tool (tool from CAM)

with limiting surfaces

Tool with smaller radius

Machining surface, inner surface

Limiting surface of pocket floor

Compensation in relation to machining

surface

Compensation in relation to limiting

surface

The control recognizes the fact that it is not

just a question of compensating in the

machining surface direction

, but also of

making an adjustment in the tool direction

, so that the point of action (green) is at the

same level as the pocket floor. This results in

a shift in the cutter tip (blue) in the direction of

the pocket floor.

This compensation variant is called Circumferential milling with limiting surfaces. It is

selected via the code CUT3DCC or CUT3DCCD and activated with G41/42 as for CUT3DC.

With CUT3DCC, the coordinates in the NC program refer to the contour and consequently the full

miller radius is compensated. For the compensation radius this results in R = $TC_DP6 plus the

programmable offset that is defined by OFFN=…., and for the face milling on the floor, the corner

radius $TC_DP7. This results in R' = $TC_DP6 + $TC_DP15 + OFFN for the circumferential

milling component and r' = $TC_DP7 + $TC_DP16 for the face milling with the other cutter side.

For CUT3DCCD, the programmed path refers to the standard tool (zero tool). The compensation

value is then the difference between the zero tool and the reground current tool, i.e. the tool wear

value from the $TC_DP15 tool data table plus the offset OFFN=….

As with face milling, the normal vector of the limiting surface must be programmed via A4, B4, C4

or A5, B5, C5. If no normal vector is programmed, the Z direction of the current coordinate

system is assumed for the CUT3DF.

126

Important functions for 3- to 5-axis machining

3.8

3.8.5

Overview of the tool types for the 3D

compensations.

The following figure shows the tool types that

are permitted in conjunction with the 3D

compensations. For the circumferential milling

(also with limiting surfaces), only cylindrical

types (top row), for face milling, also the

conical types of the bottom row.

3.8.6

Explanation of the commands

G40

Deactivation of all variants

G41

Activation for circumferential milling, compensation direction left

G42

Activation for circumferential milling, compensation direction right

G450

Circles at external corners (all compensation types)

G451

Intersection method at external corners (all compensation types)

2 ½D circumferential milling

CUT2D

2 1/2D COMPENSATION with compensation plane determined

using G17 - G19

CUT2DF

2 1/2D COMPENSATION with compensation plane determined

using a frame

3D circumferential milling

CUT3DC

Compensation perpendicular to path tangent and tool orientation.

CUT3DCD

Activating the 3D radius compensation referred to a differential

tool for circumferential milling.

ISD

The clearance between the milling tool tip (FS) and the milling tool

construction point (FH) are specified using the command ISD.

ORID

No changes in orientation in inserted circular blocks at external

corners. Orientation motion is performed in the linear blocks.

127

Important functions for 3- to 5-axis machining

3.8

ORIC

Travel path is extended by means of circles. The change in

orientation is also performed proportionately in the circle.

Face milling

CUT3DFS

Constant orientation (3-axis). Tool points in the Z direction of the

coordinate system defined via G17 - G19. Frames do not have

any effect.

CUT3DFF

Constant orientation (3-axis). Tool in Z direction of the coordinate

system currently defined via the frame.

CUT3DF

5-axis with variable tool orientation.

CUT3DFD

Activating the 3D radius compensation based on a differential tool

for face milling.

3D circumferential milling with limiting surface (combined circumferential/face milling)

CUT3DCC

CNC program relates to the contour on the machining surface.

CUT3DCCD

The CNC program relates to the tool center point path.

128

Important functions for 3- to 5-axis machining

3.8

3.8.7

Programming example for circumferential milling

A workpiece contour needs to be milled at the circumference. Programming is to be from the top

edge of the workpiece and the insertion depth ISD is to be taken into account. In the example,

compensation is performed to the right of the contour with an ISD of 20.

CUT3DC example

N100

CYCLE800(2,"TABLE",200000,57,0,0,0,0,0,0,0,0,0,1,,1)

N101

CYCLE800()

N102

G54

N103

WORKPIECE(,,"","BOX",112,0,-50,-80,0,0,100,100)

N104

T="MILLER_12"

N105

N106

S6000 M3

N108

TRAORI; activate 5-axis transformation

N109

ORIWKS; orientation reference is the WCS

N110

ORIVECT

N111

CUT3DC; 3D tool radius compensation for circumferential milling

N112

G54 G0 X-20 Y-20 D1

N113

G0 Z10

N114

G1 Z-10 F1000 M8

N115

G41 X0 A3=1.7632698 B3=0 C3=10; activate tool radius compensation to the right of the contour

and approach

N116

G1 Y100

N117

G1 A3=0 B3=-1.7632698 C3=10

N118

G1 X100

N119

G1 A3=-1.7632698 B3=0 C3=10

N120

G1 Y0

N121

G1 A3=0 B3=1.7632698 C3=10

N122

G1 X0

N123

G40 X-20 Y-20 A3=0 B3=0 C3=1; deactivate tool radius compensation and retract

N124

G0 Z100

N125

TRAFOOF

N126

M30

129

Important functions for 3- to 5-axis machining

3.9

Volumetric Compensation System (VCS)

As far as the production of large workpieces is concerned, e.g. structural parts on gantry-type

milling machines, it is very difficult to achieve the necessary level of machine positioning

accuracy due to the large dimensions of the working area. Errors due to sagging, buckling, etc. in

particular can only be remedied mechanically with a great deal of effort.

The volumetric compensation system for the SINUMERIK is a tool for correcting geometric

distortions of the machine mechanics. It reduces the effects of machine errors on the tool center

point (TCP) systematically, thereby increasing the accuracy of the machine.

Types of VCS

Below are some examples of the kinds of

compensation

error source that can be compensated:

Linear position deviation

Straightness of axes

Unintentional axis rotations

Roll, pitch, and yaw

Squareness of axes in relation to one

another

Tool orientation errors involving swivel

heads

As part of this process, the machine errors are detected on the basis of measurements and an

error file is generated. VCS then implements the compensation values automatically. To increase

the level of accuracy, calibration and testing with the compensation values can be performed

using an iterative method. VCS automatically compensates the detected errors in conjunction

with TRAORI.

As regards the VCS commissioning process and machine calibration, please contact your

machine manufacturer.

130

Important functions for 3- to 5-axis machining

3.10

VNCK - virtual machine

Due to the level of complexity and machining time associated with 5-axis milled workpieces, a

deliberate effort is made to check that the programs are free of errors before actual production

commences. To ensure that the data obtained is as realistic as possible, virtual models of the

machine and control are created and simulated. Siemens provides the following basic modules

for this purpose:

The virtual NC kernel (VNCK)

Using these basic modules and other components, such as the CAD data for the real machine,

the machine manufacturer or CAM system manufacturer can create a virtual machine that

resembles the real machine as closely as possible.

Using the virtual machine in conjunction with the SIEMENS VNCK offers many advantages:

Programming errors are detected immediately.

Program simulation with calculation of the actual time so that production effort can be

estimated more easily.

Collision checking with actual tools, clamping devices, and machine geometries.

While the current production process is underway, the workpiece can be programmed,

optimized and then implemented on the machine immediately.

Shorter setup times.

Can be used for training and instruction. New machines can be programmed without any risk.

131

SINUMERIK 840D sl. Training. Operate - Turning (2016-2020) - page 8