Fagor 8040 MC CNC, Manual

Page: 77 / 247

Chapter 2 - page 15
MC work mode
2.5.1.1 VARIABLE TOOL CHANGE POINT
If the manufacturer wishes the user can be allowed to define the tool change point at all times. This
feature logically depends on the type of machine and type of changer.
This feature allows the tool change to be made beside the part, thus avoiding movements to a change
point farther away from the same.
To allow this:
Define text 47 of the program 999997 for the CNC to request the coordinates on X, Y and Z of
the change point.
For example: ;47 $CHANGE POSITION
These coordinates should always refer to machine reference zero (home), for the zero offsets not
to affect the tool change point.
For this reason, the CNC can display, along with coordinates X, Y, Z and in small characters, the
coordinates for the axes referring to home.
For the CNC to show the coordinates of the axes referring to home text 33 of program 999997
has to be defined. For example: ;33 $REFERENCE ZERO (HOME)
Since the tool change point can be modified by the operator at any time, the subroutine associated
with the tools must take these values into account.
Arithmetical parameters P290, P291 and P292 contain the values set by the operator as change
position on X, Y, Z.
Arithmetic parameter P290
Change position on X
Arithmetic parameter P291
Change position on Y
Arithmetic parameter P292
Change position on Z
In subroutine 55 of the previous section, the line fixing the movement to the change point must be
modified:
Where it says: G0 G53 XP??? YP??? ZP??? ; Movement to the change point.
It should say: G0 G53 XP290 YP291 ZP292 ; Movement to the change point defined by
the user.
Define the coordinates of the change point (X, Y, Z)
Press key for selecting field «T». Then press key for the relevant axis
or keys:
After moving over the coordinates for the axis to be defined, one can:
a) Enter the value manually. Key in the value required and press the key
b) Assign the present position of the machine.
Move the axis, by means of the handwheel or the JOG keys, up to the point required.
Press key The CNC assigns said coordinate to the field selected.
Press key
2. Operating in JOG mode
2.5 Tool control
2.5.1 Variable tool change point