HEIDENHAIN CNC Pilot 4290 Pilot - Manual (Page 25)

25
Additive compensation G149-Geo
The CNC PILOT manages 16 tool-independent
correction values.
To activate the additive correction function, program
G149 followed by a „D number“ (for example, G149
D901). ”G149 D900” resets the additive
compensation function.
Basics of programming
■ Additive compensation is effective from the block
in which G149 is programmed.
■ An additive compensation remains active until:
• the next ”G149 D900”
• the end of the finished part description
Parameters
D:
Additive compensation - Default: D900
Range: 900 to 916
Note the direction of contour description!
Blockwise finishing allowance G52-Geo
G52 defines an equidistant finishing allowance which is taken into
consideration in G810, G820, G830, G860 and G890.
Basics of programming
■ G52 is a non-modal function.
■ G52 is programmed in the NC block containing the contour element
for which it is destined.
■ G50 before a cycle (MACHINING section) switches G52 oversizes for
this cycle off.
Parameters
P:
Finishing allowance (radius)
H: (Translation of P) absolute / additive – default: 0
■ H=0: P replaces G57/G58 allowances
■ H=1: P is added to G57/G58 allowances
Feed rate per revolution G95-Geo
G95 influences the finishing feed rate of G890.
Basics of programming
■ G95 is a modal function
■ G10 switches the G95 finishing feed rate off.
Parameters
F:
Feed per revolution
• Use peak-to-valley height and finishing feed rate alternatively.
• The G95 finishing feed rate replaces a finishing feed rate
defined in the machining program.
Help commands f
o
r
cont
our descr
iption