Interpretation Of The Programmed Path - HEIDENHAIN TNC 640 User Manual

Hide thumbs Also See for TNC 640:

Table of Contents

Multiple-Axis Machining | Peripheral Milling: 3-D radius compensation with M128 and radius compensation

Example: Definition of the tool orientation with M128 and the

coordinates of the rotary axes

N10 G00 G90 X-20 Y+0 Z+0 B+0 C+0*

N30 G01 G42 X+0 Y+0 Z+0 B+0 C+0 F1000*

N40 X+50 Y+0 Z+0 B-30 C+0*

Interpretation of the programmed path

With the FUNCTION PROG PATH function, you decide whether the

control will apply the 3-D radius compensation only to the delta

values, just as before, or rather to the entire tool radius. If you

activate FUNCTION PROG PATH, the programmed coordinates

exactly correspond to the contour coordinates. With FUNCTION

PROG PATH OFF, you deactivate this special interpretation.

Proceed as follows for the definition:

Show the soft-key row with special functions

Press the PROGRAM FUNCTIONS soft key

Press the FUNCTION PROG PATH soft key

You have the following possibilities:

Activate the interpretation of the programmed

path as the contour

The control takes the full tool radius R + DR and

the full corner radius R2 + DR2 into account for 3-

D radius compensation.

Deactivate the special interpretation of the

programmed path

The control only uses the delta values DR and

DR2 for 3-D radius compensation.

If you activate FUNCTION PROG PATH, the interpretation of the

programmed path as the contour is effective for 3-D compensation

movements until you deactivate the function.

HEIDENHAIN | TNC 640 | ISO Programming User's Manual | 10/2017

Pre-position

Activate M128

Activate radius compensation

Position the rotary axis (tool orientation)