Feed Rate In Millimeters Per Spindle Revolution: M136; Feed Rate For Circular Arcs: M109/M110/M111 - HEIDENHAIN TNC 620 User Manual

7

Feed rate in millimeters per spindle revolution: M136

Standard behavior
The control moves the tool at the feed rate F in mm/min
programmed in the NC program
Behavior with M136
In NC programs based on inch units, M136 is not allowed
in combination with FU or FZ.
The workpiece spindle is not permitted to be controlled
when M136 is active.
It is not possible to combine M136 with an oriented
spindle stop. The control cannot calculate the feed rate
because the spindle does not rotate during an oriented
spindle stop.
With M136, the control does not move the tool in mm/min, but rather
at the feed rate F in millimeters per spindle revolution programmed
in the NC program. If you change the spindle speed by using the
potentiometer, the control changes the feed rate accordingly.
Effect
M136 becomes effective at the start of the block.
You can cancel M136 by programming M137.

Feed rate for circular arcs: M109/M110/M111

Standard behavior
The control applies the programmed feed rate to the path of the tool
center.
Behavior for circular arcs with M109
For inside and outside machining of circular arcs, the control keeps
the feed rate at the cutting edge constant.
Caution: Danger to the tool and workpiece!
If the M109 function is active, the control might significantly
increase the feed rate when machining very small outside corners
(acute angles). There is a risk of tool breakage or workpiece
damage during machining.
Do not use M109 for machining very small outside corners
(acute angles)
232
Miscellaneous functions | Miscellaneous functions for path behavior
NOTICE
HEIDENHAIN | TNC 620 | Klartext Programming User's Manual | 01/2022