- Commands that can be specified during tool center point control
The commands that can be specified during tool center point control are linear
interpolation (G01), positioning (G00), circular interpolation (G02, G03), and helical
interpolation (G02, G03).
When linear interpolation (G01) is specified during tool center point control, speed
control is exerted so that the tool center point moves at the specified speed.
The circular interpolation command (G02, G03) controls the tangential speed of the
arc path along which the tool center point moves.
The helical interpolation command (G02, G03) controls the tangential speed of the arc
path along which the tool center point moves or a synthetic speed including that of the
helical axis. (This is dependent on the setting of parameter RHT (No.1407#4).)
As the actual speed, the speed at the control point is shown.
For information about the positioning command (G00), see the following CAUTION
box.
CAUTION
1 Be sure to set the following parameters.
1) Parameter LRP(No.1401#1)=1 : Rapid in straight-line
2) Parameter FRP(No.19501#5)=1 : Acceleration/deceleration
before interpolation for rapid traverse.
3) Parameter No.1773 : A time constant for acceleration before
interpolation in rapid traverse. (When parameter No.1773 is set
to 0, parameter No.1620 is effective.)
4) Parameter No.1774 : Change time for bell-shaped acceleration
before interpolation for rapid traverse.
(When parameter No.1774 is set to 0, parameter No.1621 is
effective.)
2 Alarm PS5420 occurs without one of the above settings.
- Rotation axis command
If a command is specified during tool center point control that has no movement of the
tool center point with respect to the workpiece, the maximum cutting speed
(parameter No.1422 or 1430 or 1432) is assumed as the feedrate of the rotation axis
when parameter RFC (No.19696#6) is 0, and the speed specified by F is assumed
when parameter RFC (No.19696#6) is 1.
The rotation axis command cannot be specified during tool center point control of
type 2. Specifying the command with type 2 causes alarm PS5421.
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
28/28