Fagor 8055 EN, Programming Manual

Page: 154 / 482

·154·
Programming manual
CNC 8055
CNC 8055i
9.
CANN
ED
CYCLES
·M· & ·EN· M
ODELS
S
OFT
: V02.2
X
Mach
inin
g canne
d cycl
es
9.5 Machining canned cycles
In all machining cycles there are three coordinates along the longitudinal axis to the work plane
which, due to their importance, are discussed below:
• Initial plane coordinate. This coordinate is given by the position which the tool occupies with
respect to machine zero when the cycle is activated.
• Coordinate of the reference plane. This is programmed in the cycle definition block and
represents an approach coordinate to the part. It can be programmed in absolute coordinates
or in incremental, in which case it will be referred to the initial plane.
• Machining depth coordinate. This is programmed in the cycle definition block. It can be
programmed in absolute coordinates or in incremental coordinates, in which case it will be
referred to the reference plane.
There are two functions which allow to select the type of withdrawal of the longitudinal axis after
machining.
• G98: Selects the withdrawal of the tool as far as the initial plane, once the indicated machining
has been done.
• G99: Selects the withdrawal of the tool as far as the reference plane, once the indicated
machining has been done.
These functions can be used both in the cycle definition block and the blocks which are under the
influence of the canned cycle. The initial plane will always be the coordinate which the longitudinal
axis had when the cycle was defined.
The structure of a canned cycle definition block is as follows:
It is possible to program the starting point in the canned cycle definition block (except the longitudinal
axis), both in polar coordinates and in Cartesian coordinates.
After defining the point at which it is required to carry out the canned cycle (optional), the functions
and parameters corresponding to the canned cycle will be defined, and afterwards, if required, the
complementary functions F S T D M are programmed.
When programming, at the end of the block, the number of times a block is to be executed "N", the
CNC performs the programmed move and the machining operation corresponding to the active
canned cycle the indicated number of times.
If "N0" is programmed, it will not execute the machining operation corresponding to the canned cycle.
The CNC will only carry out the programmed movement.
The general operation for all the cycles is as follows:
1. If the spindle was previously running, it maintains the turning direction. If it was not in movement,
it will start by turning clockwise (M03).
2. Positioning (if programmed) at the starting point for the programmed cycle.
3. Rapid movement of the longitudinal axis from the initial plane to the reference plane.
4. Execution of the programmed machining cycle.
5. Rapid withdrawal of the longitudinal axis to the initial plane or reference plane, depending on
whether G98 or G99 has been programmed.
The explanation of each cycle assumes that the work plane is formed by the X and Y axes, and
that the longitudinal axis (perpendicular) is the Z axis:
G** Machining point Parameters F S T D M N****