G84. Tapping canned cycle. Fagor CNC 8055 para otras aplicaciones, CNC 8055 para fresadoras, CNC 8055 for milling machines, CNC 8055 for other applications

9.

Programming manual

9.10

G84. Tapping canned cycle

This cycle taps at the point indicated until the final programmed coordinate is reached. General logic output "TAPPING" (M5517) stays active while executing this cycle.

Due to the fact that the tapping tool turns in two directions (one when tapping and the other when withdrawing from the thread), by means of the machine parameter of the spindle "SREVM05" it is possible to select whether the change in turning direction is made with the intermediate spindle stop, or directly.

General machine parameter "STOPAP(P116)" indicates whether general inputs /STOP, /FEEDHOL and /XFERINH are enabled or not while executing function G84.

It is possible to program a dwell before each reversal of the spindle turning direction, i.e., at the bottom of the thread hole and when returning to the reference plane.

Using parameters B and H, the threading may be done with relief for chip breakage.

The tapping with relief is done in successive approaches until the programmed total depth is reached. After every approach, it withdraws for chip relief. In this case, the dwell (K) is only applied on the last pass, not on the relief passes.

Working in Cartesian coordinates, the basic structure of the block is as follows:

G84 G98/G99 X Y Z I K R J B H

CNC 8055

CNC 8055i

·M· & ·EN· M ODELS

S OFT : V01.6

X

[ G98/G99 ] Withdrawal plane

G98 The tool withdraws to the Initial Plane, once the hole has tapped.

G99 The tool withdraws to the Reference Plane, once the hole has tapped.

[ X/Y±5.5 ] Machining coordinates

These are optional and define the movement of the axes of the main plane to position the tool at the machining point.

This point can be programmed in Cartesian coordinates or in polar coordinates, and the coordinates may be absolute or incremental, according to whether the machine is operating in G90 or G91.

[ Z±5.5 ] Reference plane

Defines the reference plane coordinate. It can be programmed in absolute coordinates or incremental coordinates, in which case it will be referred to the initial plane.

If not programmed, it assumes as reference plane the current position of the tool.

[ I±5.5 ] Thread depth.

Defines tapping depth. It can be programmed in absolute coordinates or incremental coordinates and in this case will be referred to the reference plane.

[ K5 ] Dwell

Defines the dwell, in hundredths of a second, after the tapping until the withdrawal begins. If not programmed, the CNC will take the value of "K0".

·168·

Programming manual

[ R ] Type of tapping

Defines the type of tapping to be carried out.

R0 Normal tapping.

R1

R2

Rigid tapping. The CNC stops the spindle with M19 and orients it to begin tapping.

Rigid tapping. If the spindle is turning in M3 or M4, the CNC does not stop it nor orient it to begin tapping. This option does not allow thread repair, even if the part has not been released because the thread start (entry) will coincide with the one machined earlier.

[ J5.5 ] Withdrawal feedrate factor

When rigid tapping, the returning feedrate will be J times the tapping feedrate. When not programmed or programmed J1, they will both be the same.

In order to execute a rigid tapping, the spindle must be ready to operate in closed loop; in other words, that it must have a servo drive-motor system with rotary encoder.

When rigid tapping, the CNC interpolates the movement of the longitudinal axis with the spindle rotation.

[ B5.5 ] Penetration step during tapping with relief.

It is optional and sets the penetration step during tapping with relief. This parameter is ignored when programming R=0 or R=2. Tapping with relief is only possible when programming R=1.

When not programmed, tapping will be done in a single pass. When programmed with a 0 value, it issues the corresponding error.

[ H5.5 ] Withdrawal distance after each penetration step.

This withdrawal will be done at a speed that will take into consideration the factor programmed in

J. This parameter is ignored when programming R=0 or R=2, or if parameter B has not been programmed.

If not programmed or programmed with a 0 value, the withdrawal will be done to the Z reference plane coordinate.

9.

CNC 8055

CNC 8055i

·M· & ·EN· M ODELS

S OFT : V01.6

X

·169·