- Positioning and linear interpolation for tool center point control (type 2)
G43.5 IP
H Q ; Starts tool center point control (type 2).
IP
I J K ;
:
IP : In the case of an absolute command, the coordinate value of the
end point of the tool tip movement
In the case of an incremental command, 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
H : Tool offset number
Q : 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 along the tool axis direction.
No rotation axes are specified. Instead, the direction of the tool end point is specified
as I, J, K, as seen from the programming coordinate system.
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 mixed type machine, however, these cannot be
specified at the block of G43.5. Specifying them with a table rotation type or mixed
type machine causes alarm PS5421.
While the rotation axes are moving, 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 Type 2 can be used only when the programming coordinate system is
fixed on the table (when the WKP parameter (No.19696#5) is set to
0). Specifying G43.5 when the WKP parameter (No.19696#5) is set to
1 causes alarm PS5459.
4 Type 2 cannot be used when there is only one rotation axis or when
any virtual axis is used. Specifying G43.5 in such a case causes alarm
PS5459.
5 When using the rotation axis rollover function, set parameter No.1260
(amount of movement per rotation of the rotation axis) to 360 degrees.
B-63534EN/02-05
Edit
Apprv. Desig.
Sheet
Title
Draw
No.
Date
Design
Description
Date
FANUC Series 16i/160i/160is-MB,18i/180i/180is-MB5,
18i/180i/180is-MB OPERATOR’S MANUAL
Concerning the addition of TOOL CENTER POINT
CONTROL FOR 5-AXIS MACHINING
Oct.27.2003
T. Horie
10/10