Brother TC-32B - Helical Interpolation

Chapter 3 Preparation Function TC-32B
2004/01/22 3 - 20 eTCOMNCPR3.doc
3
3.4.2 Helical interpolation
Putting the other than selected plane axis command in the circular arc block permits a helical
cutting.
Command format
X-Y plane:
G17G02 X_Y_Z_ I_ J_ F_;
R_
G17G03 X_Y_Z_ I_ J_ F_;
R_
Z-Y plane:
G18G02 Z_X_Y_ K_I_ F_;
R_
G18G03 Z_X_Y_ K_I_ F_;
R_
Y-Z plane:
G19G02 Y_Z_X_ J_K_ F_;
R_
G19G03 Y_Z_X_ J_K_ F_;
R_
The F code commands the feedrate in the circular interpolation axis..
If the value of F is larger than the MAXIMUM CUTTING SPEED or the FEEDRATE SPEED set
by the machine parameter, an alarm is generated.
The feedrate in the other than selected plane axis is determined by the values of "feedrate" in the
circular interpolation axis, "end point X", "end point Y" and "end point Z". It can be calculated as
follows:
180
× L
F
Z
= × F
π × R × θ
F: Command speed (X, Y axes)
R: Radius (Start point, center)
θ:Angle
Fz: Other than selected plane of feeedrate speed.
L: Other than selected plane of feeed distance.
Ex.)
Setting following values:
F=500 (mm/min), R=10 (mm), θ=360 (°), L=2 (mm)
Fz = (180×2×500)/(
π×10×360) 15.9 (mm/min)
If the other than selected plane axis feedrate is larger than the MAXIMUM CUTTING SPEED or
FEEDRATE SPEED set by the machine parameter , an alarm is generated.
When tool dia offset command is given, an offset is applied to the selected plane.
.
.
=