HEIDENHAIN iTNC 530 (340 422) - Manual (Page 506)

506 11 Programming: Q Parameters
1
1
.1 Pr
inciple and Ov
erview
11.1 Principle and Overview
You can program an entire family of parts in a single part program. You
do this by entering variables called Q parameters instead of fixed
numerical values.
Q parameters can represent information such as:
„ Coordinate values
„ Feed rates
„ Spindle speeds
„ Cycle data
Q parameters also enable you to program contours that are defined
with mathematical functions. You can also use Q parameters to make
the execution of machining steps depend on logical conditions. In
conjunction with FK programming you can also combine contours that
do not have NC-compatible dimensions with Q parameters.
Q parameters are designated by the letter Q and a number between 0
and 399. They are grouped according to three ranges:
Programming notes
You can mix Q parameters and fixed numerical values within a
program.
Q parameters can be assigned numerical values between –
99 999.9999 and +99 999.9999. Internally, the TNC can calculate up to
a width of 57 bits before and 7 bits after the decimal point (32-bit data
width corresponds to a decimal value of 4 294 967 296).
Meaning Range
Freely applicable parameters, globally effective
for all programs stored in the TNC memory Q0 to Q99
Parameters for special TNC functions Q100 to Q199
Parameters that are primarily used for cycles,
globally effective for all programs that are stored
in the TNC memory Q200 to Q399
Q4
Q2
Q3 Q1
Q5
Q6
Some Q parameters are always assigned the same data by
the TNC. For example, Q108 is always assigned the
current tool radius (see “Preassigned Q Parameters” on
page 540).
If you are using the parameters Q60 to Q99 in encoded
OEM cycles, define via MP7251 whether the parameters
are only to be used locally in the OEM cycles (.CYC file), or
may be used globally.