FANUC Series 30i/300i/300is-MODEL A. Machining Center System. User's manual - page 102

22.5-AXIS MACHINING FUNCTION

PROGRAMMING

B-63944EN/03

- 772 -

5-AXIS MACHINING FUNCTION

Chapter 22, "5-AXIS MACHINING FUNCTION", consists of the
following sections:

22.1  TOOL CENTER POINT CONTROL ....................................773
22.2  TOOL POSTURE CONTROL ...............................................828
22.3  TILTED WORKING PLANE COMMAND..........................838
22.4  INCLINED ROTARY AXIS CONTROL..............................894
22.5  3-DIMENSIONAL CUTTER COMPENSATION ................897

B-63944EN/03

PROGRAMMING

22.5-AXIS MACHINING FUNCTION

- 773 -

22.1

TOOL CENTER POINT CONTROL

Overview

On a 5-axis machine having two rotary axes that turn a tool or table,
this function performs tool length compensation constantly, even in
the middle of a block, and exerts control so that the tool center point
moves along the specified path. (See

Fig. 22.1 (a).)

There are three different types of 5-axis machines - <1> those that
rotate the tool only, <2> those that rotate the table only, and <3> those
that rotate both the tool and table.    (See Fig. 22.1 (d).)
This function is intended to perform machining on such 5-axis
machines having rotary axes that turn a tool or table as well as three
orthogonal axes (X-, Y-, and Z-axes) by accomplishing tool length
compensation while changing the attitude of the tool.    It enables the
tool center point to move along the specified path even if the tool's
direction changes with respect to the workpiece.
A coordinate system used for programming the tool center point
control is called the programming coordinate system.
A coordinate system fixed on the table can be used as the
programming coordinate system, which makes CAM programming
easy. This coordinate system is particularly called the table
coordinate system.
A workpiece coordinate system fixed on a machine coordinate system
can be employed as the programming coordinate system as well.
In any case, the cutting speed can be controlled easily because the tool
center point moves at a specified speed with respect to the table
(workpiece).
The commands that can be issued during tool center point control are
positioning (G00), linear interpolation (G01), circular interpolation
(G02, G03), and helical interpolation (G02, G03).

Program-specified
path

Control
point

Tool length
vector

Tool center
point

Fig. 22.1 (a) Path of the tool center point

22.5-AXIS MACHINING FUNCTION

PROGRAMMING

B-63944EN/03

- 774 -

Tool center point path

Fig. 22.1 (b) Path of the tool center point

B-63944EN/03

PROGRAMMING

22.5-AXIS MACHINING FUNCTION

- 775 -

When a coordinate system fixed on the table is used as the
programming coordinate system, programming can be performed
without worrying about the rotation of the table because the
programming coordinate system does not move with respect to the
table, although the position and direction of the workpiece fixed on
the table change due to its rotation.    When a straight line is specified,
the tool center point moves along a straight path with respect to the
workpiece as instructed.    (See Fig. 22.1 (b).)
By setting the relevant parameter, the workpiece coordinate system
can also be employed as the programming coordinate system.    In this
case, as the table turns, the position and direction of the workpiece
fixed on the table change with respect to the programming coordinate
system.    It is therefore necessary to take into account the rotation of
the table when specifying the end point.  In this case, too, when a
straight line is specified, the tool center point moves along a straight
path with respect to the workpiece as instructed.
Fig. 22.1 (c) illustrates how linear interpolation is accomplished with a
composite type machine, showing the relationship between the case
when a table-fixed coordinate system is used as the programming
coordinate system and the case when the workpiece coordinate system
is used.  If linear interpolation is specified in this function mode,
speed control is exerted in such a way that the tool center point moves
at a specified speed with respect to the workpiece.

Example)
Machine configuration: The A-axis is the rotation axis for controlling the tool.

The B-axis is the rotation axis for controlling the table.

Program: Created using the programming coordinate system.

Workpiece coordinate
system used when tool
center point control starts

Specified
start point

Specified end-point vector resulting when
a table-fixed coordinate system is used as
the programming coordinate system

The cutting path is straight

Workpiece
coordinate
system (It
doesn’t move
even if the

B-axis rotates.)

Specified end-point vector resulting when
a workpiece coordinate system is used as

the programming coordinate system

X”

Y”

Coordinate system fixed on the table

X”

Y”

Fig. 22.1 (c) Linear interpolation with a composite type machine

22.5-AXIS MACHINING FUNCTION

PROGRAMMING

B-63944EN/03

- 776 -

<2> Table rotation type machine

<3> Composite type machine

<1> Tool rotation type machine

Fig. 22.1 (d) Three types of 5-axis machine

Even if the rotary axis that controls the tool does not intersect the one
that controls the table, this function can still be used.

B-63944EN/03

PROGRAMMING

22.5-AXIS MACHINING FUNCTION

- 777 -

There are two types, as described below, one of which is used
depending on how the direction of the tool axis is specified.

(1) Type

The block end point of the rotary axes is specified (e.g. A, B, C).

The CNC performs tool length compensation by the specified
amount in the tool axis direction that is calculated from the
specified position of the rotary axes and exerts control so that the
tip of the tool moves along the specified path.

(2) Type

The direction of the tool axis (I, J, K) at the block end point, as
seen from the coordinate system fixed on the table, is specified,
instead of the position of the rotary axes.

The CNC calculates an end point of the rotary axes where the
tool will face the specified direction, performs tool length
compensation by the specified amount in the tool axis direction
that is calculated from the position of the rotary axes, and exerts
control so that the tip of the tool moves along the specified path.

Format
- Positioning and linear interpolation for tool center point control (type 1)

G43.4

_ H_ ;

Starts tool center point control (type 1).

_ ;

: In the case of an absolute programming, the coordinate

value of the end point of the tool tip movement

In the case of an incremental programming, the amount of

the tool tip movement

: In the case of an absolute programming, the coordinate

value of the end point of the rotary axes

In the case of an incremental programming, the amount of

the rotary axis movement

H : Tool offset number

Movement to the position specified by the G43.4 block (startup) does
not constitute tool center point control. Only tool length
compensation is performed.
As for rotary axes, either table rotation axes or tool rotation axes are
specified.

While performing interpolation for the rotary axes, the CNC controls
the control points so that the tool center point moves along a straight
line with respect to the table (workpiece). The end of the tool center
point comes to the point specified on the programming coordinate
system.

22.5-AXIS MACHINING FUNCTION

PROGRAMMING

B-63944EN/03

- 778 -

- Positioning and linear interpolation for tool center point control (type 2)

G43.5

_ H_ Q_ ;

Starts tool center point control (type 2).

_ I_ J_ K_ ;

: In the case of an absolute programming, the

coordinate value of the end point of the tool tip
movement

In the case of an incremental programming, the

amount of the tool tip movement

I, J, K : Tool axis direction at the block end point as seen from

the programming coordinate system

: Tool offset number

: Inclination angle of the tool (in degrees)

Movement to the position specified by the G43.5 block does not
constitute tool center point control.    Only tool length compensation is
performed.
No rotary axes are specified.  Instead, the direction of the tool end
point is specified as I, J, K, as seen from the programming coordinate
system (the one fixed on the table when G43.5 is specified).
With a tool rotation type machine, I, J, K can be specified using the
G43.5 block.    In the case of a table rotation type or composite type
machine, however, these cannot be specified.    Specifying them with
a table rotation type or composite type machine causes alarm PS5421.

While performing interpolation for the rotary axes, the CNC controls
the control points so that the tool center point moves along a straight
line with respect to the table (workpiece).    The end of the tool center
point comes to the point specified on the programming coordinate
system.

CAUTION

1 If one or two of the I, J, and K values are omitted, the

omitted value or values are considered to be 0.

2 In a block in which I, J, and K are all omitted, the

compensation vector of the preceding block is used.

3 This block can be used only when the programming

coordinate system is fixed on the table (when the bit 5
(WKP) of parameter No.19696 is set to 0). Specifying
G43.5 when bit 5 (WKP) of parameter No.19696 is set
to 1 causes alarm PS5459.

4 Type 2 cannot be used when there is only one rotary

axis or when any hypothetical axis is used. Specifying
G43.5 in such a case causes alarm PS5459.

5 When using the rotary axis rollover function or the

rotary axis control function, set parameter No.1260
(amount of movement per rotation of the rotary axis) to
360 degrees.

B-63944EN/03

PROGRAMMING

22.5-AXIS MACHINING FUNCTION

- 779 -

- Circular interpolation for tool center point control (type 1)

G43.4

_ H_ ;

Starts tool center point control (type 1).

G17  : X-Y plane of the table coordinate system
G18  : Z-X plane of the table coordinate system
G19  : Y-Z plane of the table coordinate system
G02  : Clockwise (CW) circular interpolation
G03  : Counterclockwise (CCW) circular interpolation

: In the case of an absolute programming, the

coordinate value of the end point of the tool tip
movement

In the case of an incremental programming, the

amount of the tool tip movement

(This pertains only to two axes on the plane.)

I, J, K : Specify the distance between the start point in the

rotary axis position of the block start point and the
center of the arc, as seen from the programming
coordinate system.

: Arc radius R > 0: The center angle of the arc is less

than 180°.

R < 0: The center angle of the arc is

more than 180

: In the case of an absolute programming, the

coordinate value of the end point of the rotary axis

In the case of an incremental programming, the

amount of the rotary axis movement

: Specified speed (speed in the tangent direction of the

arc as seen from the table coordinate system)

: Tool offset number

Movement to the position specified by the G43.4 block does not
constitute tool center point control.    Only tool length compensation is
performed.  While performing interpolation for the rotary axes, the
CNC controls the control points so that the tool center point moves
along an arc with respect to the table (workpiece).  The end of the
tool center point comes to the point specified on the programming
coordinate system.

CAUTION

Any command that does not move the tool center point
with respect to the workpiece (one that moves the rotary
axes only) must be executed in G00 or G01 mode.

G02

J K

G17

F ;

G03

G02

J K

G18

F ;

G03

G02

J K

G19

F ;

G03

Content .. 100 101 102 103 ..