HEIDENHAIN CNC Pilot 4290 - Manual (Page 106)

4 DIN PLUS 94
Feed per revolution G95-Geo
Influences the finishing feed rate of G890.
Parameters
F:
Feed per revolution
Programming notes
■ G95 is a modal function.
■ G10 resets a finishing feed rate set with G95.
Additive compensation G149 Geo
The CNC PILOT manages 16 tool-independent compensation values.
To activate the additive compensation function, program G149
followed by a ”D number” (for example, G149 D901). ”G149 D900”
resets the additive compensation function.
Parameters
D:
Additive compensation – default: D900 – range: 900 to 916
Programming notes
■ Additive compensation is effective from the block in
which G149 is programmed.
■ An additive compensation remains effective until:
■ The next ”G149 D900”.
■ The end of the finished part description.
Note the direction of contour description!
Programming notes
■ G52 is a non-modal function.
■ G52 is programmed in the NC block containing the
contour element for which it is destined.
■ G50 preceding a cycle (MACHINING section)
cancels a finishing allowance programmed for that
cycle with G52.
Blockwise oversize G52-Geo
Equidistant allowance that is taken into consideration in G810, G820,
G830, G860 and G890.
Parameters
P:
Finishing allowance (radius)
H: (Translation of P) absolute / additive – default: 0
■ H=0: P replaces G57/G58 oversizes
■ H=1: P is added to G57/G58 oversizes
■ 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.
4.5 Geometry Commands