HEIDENHAIN SW 68894x-02 - Manual (Page 591)

HEIDENHAIN CNC PILOT 640 591
9.4
Compatibility
in
DIN
pr
ogr
ams
9.4 Compatibility in DIN programs
The format of DIN programs of the CNC PILOT 4290 predecessor
control differs from the format of the CNC PILOT 640. However, you
can use the program converter to adapt programs of the predecessor
control to the new control.
When opening an NC program, the CNC PILOT 640 recognizes the
programs of the predecessor control. The program concerned will be
converted after a confirmation prompt. "CONV_..." will be prefixed to
the program name. The program converter is also part of the Transfer
function (Organization mode of operation).
When converting DIN programs, it is also important to keep in mind
that the predecessor controls use different solutions for tool
management, parameter management, programming with variables
and PLC programming.
Remember the following when converting DIN programs of the CNC
PILOT 4290:
Tool call (T commands of the TURRET section):
 T commands containing a reference to the tool database are left
unchanged (example: T1 ID“342-300.1“)
 T commands containing tool data cannot be converted
Programming variables
 D variables (# variables) are replaced by # variables of the new
syntax. Depending on the range of numbers, #c or #l or #n or #i
variables will be used.
 Special conversion rules: #0 is converted to #c30, #30 is converted
to #c51
 V variables are replaced by #g variables. Braces used in assignments
are removed. Braces used in expressions are changed to
parentheses.
 Variable accesses to tool data, machine dimensions, D
compensation values, parameter data and events cannot be
converted. These program sequences have to be adapted.
Exception: The "Mid-program startup active" E90[1] event is
converted to #i6
 Remember that – unlike the 4290 – the interpreter of the CNC PILOT
640 re-evaluates the lines every time the program is executed.
M functions:
 M30 with NS.. is converted to M0 M99 NS
 M97 is removed for single-channel controls
 All other M functions are left unchanged.
G functions:
 The following G functions are currently not supported by the CNC
PILOT 640: G48, G53, G54, G55, G62, G63, G98, G162, G204,
G710, G906, G907, G915, G918, G975, G995, G996
 A warning will be issued if the following G functions are used in a
contour description: G10, G38, G39, G52, G95, G149. These
functions are now modal.