
2. MACHINING PROGRAMS FOR
LATHES WITH C–AXIS
B–62444E–1/04
TYPES OF MACHINING
PROGRAMS
412
NOTE
1 The rewriting of the above cutter compensation data is
executed with the G10 instruction for each in–feed
machining operation. At that time, cutter compensation C
is made using new cutter compensation data, so a T–code
is used each time.
This means that consideration is required for the machine
to perform no operation for the same T–code.
The offset used for the processing described above is 16, 32, 64, or
97, according to the number of offset sets, so as not to destroy the
original offset data.
Therefore, the above offset numbers cannot be used in any processes
including notching.
However, when a cutting allowance of 0 is specified, cutter
compensation data is not rewritten by G10 and T–code is not output.
(3) Chamfering for notching for end faces is performed as described
below.
The Z–coordinate, CZ, of the chamfering tool tip is calculated
according to the following expression:
CZ = ZS – (C/tan(A/2) + CC)
Where CC is the tip clearance of a chamfering tool registered in the
tool file.
As with rough machining, cutter compensation C is used for
chamfering after cutter compensation data is temporarily rewritten.
Cutter compensation data for chamfering is calculated according to
the following expression:
CL = M/2 + CC
*
tan(A/2)
(4) Polar coordinate interpolation, which is an NC function, is used for
C–axis notching.
NOTE
2 Polar coordinate interpolation, which is an NC function, is
used for C–axis notching for end faces. So the restrictions
that apply to the function also apply.
For detailed information, refer to the description of polar coordinate
interpolation in the operator’s manual of the NC.