HEIDENHAIN CNC Pilot 4290 - Manual (Page 375)

HEIDENHAIN CNC PILOT 4290 363
7.5 Mac
hining P
a
ra
met
ers
5 – Finishing
Finishing – Tool and Machining Standards
Finishing tools are defined according to machining location and main
machining direction (MMD) via setting angle and point angle. For tool
selection, the following additionally applies:
■ Finishing cycles are primarily executed with standard finishing
tools.
■ If form elements such as recesses (type FD) and undercuts (type
E, F, G) cannot be machined with a standard finishing tool, one form
element after the other is skipped. TURN PLUS starts a renewed
attempt to machine the remaining contour with the standard tool.
Subsequently, the skipped form elements are machined individually
with a suitable finishing tool.
■ Setting angle – external/longitudinal [FALEW]
■ Point angle – external/longitudinal [FALSW]
■ Setting angle – external/transverse [FAPEW]
■ Point angle - external/transverse [FAPSW]
■ Setting angle – internal/longitudinal [FILEW]
■ Point angle - internal/longitudinal [FILSW]
■ Setting angle – internal/transverse [FIPEW]
■ Point angle - internal/transverse [FIPSW]
Roughing – Machining cycles
■ Overhang length - external [ULA]: Relative length for external
rough-machining enabling roughing beyond the target position in
longitudinal direction. Not considered when the cutting limitation is
in front of or within the overhang.
■ Overhang length inside [ULI] (see also ” 6.15.5 Inside Contours”)
■ Length of roughing beyond the target point during inside
machining in longitudinal direction. Not considered when the cutting
limitation is in front of or within the overhang.
■ ULI is used to calculate the drilling depth for centric predrilling.
■ Retracting length - external [RAHL]
■ Retracting length - internal [RIHL]
Retracting length for smoothing variants (H=1, 2) of roughing cycles
G810 and G820 for external machining (RAHL) / internal machining
(RIHL).
■ Cutting-depth reduction factor [SRF] – For rough-machining with
tools machining opposite to the main machining direction, the infeed
value (cutting depth) is reduced. Calculation of infeed (P) for
roughing cycles (G810, G820):
P = ZT * SRF (ZT: Infeed from the technology database)