Feed rate compensation on circular arcs(Heidenhain iTNC530,TNC640)

Standard case

The feedrate specified in CNC program refers to the path described by the tool center.For straight line movements,the feed rate of cutting point of the tool is equal to the feed rate of the center of the tool.In the case of movement on a circular arcs ,this is not true.

It can bee seen that during the machining along on circular arc(circular pocket,circular stud) not feed rate programmed by us appear at the cutting edge of the tool number.It will be higher on the inner and lower on the outside arcs.If you want that the cutting edge works at the feed rate you have programmed,you must change the feed rate of the tool center.For this the Heidenhain control uses codes M109, M110 and M111.

Programming

M109,M110,M111

Meaning of the commands

The following commands are only effective with tool radius compensation(RL,RR) is switched on !!!

M109 – The programmed feed rate will be activated on the cutting edge of the tool during the machining on both the inner and outer contours.The feed rate of the tool center decreases on the inner arc while increasing on outside arc.

M110 -The programmed feed rate will be only actived at the cutting edge of the tool when it machines the inner arc contour.The feed rate of the tool center decreases at the inside (concave) arc,while on outside(convex) arc it is the same as programmed.

M111 -The programmed feed rate for travesing on the both the outer and inner arcs is the same as the feed rate for the tool center.There is no feed sompensation on the contours,this function is default setting and cancels the functions M109,M110.

Thefeed rate of the cutting edge on the both the outer and inner arcs is the same as programmed M109,M109.

The programmed feed rate will appear at the cutting edge of the tool,resulting in zhe following:

Outside arc: F tool center>F program

Inside arc: F tool center<F program

Problem: On the external arcs,the feed rate of the tool center can increase greatly,which can also lead to tool breakage in case of higher allowance.It means the lower difference between the tool radius and arc radius the lager feedtrate of the tool center.THE SOLUTION M110

The feed rate of cutting edge only on inner arcs is the same as programmed M110.

When the cutter tool machines the inner arc of the contour,the programmed feedrate will be actived at the cutting edge of the tool. The feedrate of the center of the cutter tool on the outer arcs is the same programmed.

No feedrate compensation on arcs M111

The programmed feed rate for travesing on the both the outer and inner arcs is the same as the feed rate for the tool center.The result is as follows.

Outside arc: F prog>F cutting

Inside arc: F prog<F cutting

This is default setting for Heidenahin control.

The control display always shows the feed rate of the tool center.

For iTNC 530 control,if you enter M109 or M110,before calling a number of machining cycles higher than 200,the set feed rate will also be applied to the circular arcs within the machining cycles.After completing or interrupting the machining cycle,the initial state is restored.

Exceptions to this are the sl(cycl def 22-24) and thread milling(cycl def 262-267) cycles as the control automatically applies the feed rate compensation for these cycles.

In case of the TNC640 control,you can program feedrate comp with Q349(feedrate reference) parameter for CYCL DEF252,253,254.

For the other cycles CYCL DEF256,257,258 the M109 or M110 can be also applied for feedrate compensation.