Entering Tool-Related Data; Feed Rate F - HEIDENHAIN TNC 640 User Manual

6
6.1

Entering tool-related data

Feed rate F

The feed rate F is the speed at which the tool center point moves.
The maximum feed rates can be different for the individual axes
and are set in machine parameters.
Input
You can enter the feed rate in the TOOL CALL block and in every
positioning block.
Further information:
function keys", page 286
You enter the feed rate F in mm/min in millimeter programs, and in
1/10 inch/min in inch-programs, for resolution reasons. Alternatively,
with the corresponding soft keys, you can also define the feed rate
in mm per revolution (mm/1) FU or in mm per tooth (mm/tooth) FZ.
Rapid traverse
If you wish to program rapid traverse, enter F MAX. To enter FMAX,
press the ENT key or the FMAX soft key when the dialog question
FEED RATE F = ? appears on the control's screen.
To move your machine at rapid traverse, you can
also program the corresponding numerical value,
e.g. F30000. Unlike FMAX, this rapid traverse remains
in effect not only in the individual block but in all blocks
until you program a new feed rate.
Duration of effect
A feed rate entered as a numerical value remains in effect until a
block with a different feed rate is reached. FMAX is only effective in
the block in which it is programmed. After the block with F MAX is
executed, the feed rate will return to the last feed rate entered as a
numerical value.
Changing during program run
You can adjust the feed rate during the program run with the feed
rate potentiometer F .
The feed rate potentiometer lowers the programmed feed rate, not
the feed rate calculated by the control.
238
"Creating the NC blocks with the path
HEIDENHAIN | TNC 640 | Conversational Programming User's Manual | 10/2017
Tools | Entering tool-related data