Taping Without Encoder G63; Taping Without Compensating Chuck (Sinumerik 880 Ga2) - Siemens SINUMERIK 880 Programming Manual

4 Programming of Motion Blocks
4.3.4 Tapping without encoder G63
4.3.4 Tapping without encoder G63
The "Tapping without encoder" function is an Option.
It is an integral part of spindle package E40-E45.
Preparatory function G63 is used to tap threads using a tap in the compensating chuck. There
is no functional relationship between the spindle speed and the feedrate.
The spindle speed is programmed under address S and a suitable feedrate under address F.
The length compensating chuck must allow for the tolerances between the feedrate and the
speed as well as the spindle overrun when the position is reached.
With G63 the feedrate override switch is set to 100%. The spindle may also be stopped in
conjunction with "Feed hold" depending on the design of the interface control. The spindle
speed override switch is active only after it has been enabled by the machine data.
G63 can only be used in blocks with linear interpolation G01.
4.3.5 Tapping without compensating chuck (SINUMERIK 880 GA2)
The function, "Tapping without compensating chuck"
With this function, the compensating chuck usually required for tapping is not needed. The
function is selected and deselected with G commands. When the function is selected, the
spindle switches to rotary axis operation for which the spindle must already be in the correct
gear stage.
G203 To select rotary axis operation, clockwise (modal)
G204 To select rotary axis operation, counter-clockwise (modal)
G205 To change from rotary axis operation to spindle operation M05 (initial setting)
You must not program any other G functions, preparatory functions or auxiliary functions in
blocks containing G203/G204. You must program the rotary axis, the infeed axis and spindle
speed. The rotary axis must be programmed before the infeed axis. The rotary axis is
positioned in rapid traverse; the zero offset and tool compensation are calculated automatically.
You can only switch to this function with G203/G204 from the initial setting (G205). You must
program G205 on its own in a block. Once you have selected the function with G203/G204,
you can then program cycle L84. The cycle is supplied with parameters from R parameters R2
to R10.
N0080 G203 C45
4–62
requires the spindle package E40-E45.
The order code is E36.
Z S250
Spindle speed
Infeed axis
Rotary axis with angle
Selects rotary axis operation, clockwise
operation
© Siemens AG 1991 All Rights Reserved
01.93
6ZB5 410-0HD02
SINUMERIK 880, (PG)