Lenze ETC Motion Control - Manual (Page 116)

CNC programming
G functions
G functions individual descriptions
3
3.2
3.2.2
l
116 EDSTCXN EN 2.0
3.2.2.22 G41 Tool path correction − left, G42 Tool path correction − right
Switching on the tool radius compensation or an application−specific
correction procedure for the tool path.
G41 R J L
G42 R J L
R Tool radius to be compensated
J Tool orientation (value 0 ... 9)
L Transfer type 0: linear, 1: circular
The preparatory functions switch on the tool radius compensation or an
application−specific correction procedure. The tool radius is transferred from
the parameter field (P700), which is preset with a T change−over or can
possibly be programmed directly with the code letter R. In the case of
application−specific corrections, the dimensions are transferred via agreed
interfaces (parameter field, machine constants). G41 activates a correction
to the left, G42 to the right of the programmed path, related to the direction
of the tool movement. The compensation applies to the selected plane (G17,
G18, G19). After the compensation has been selected, the compensated
path is approached with the following block. The starting point of this block
is the current actual position, the target point lies on the compensated path
(intersection point with following block).
Refer to the following table for the corresponding tool orientation J. It shows
the relation between the coordinates of the cutting center (Xs,Ys) and the
coordinates of the tool cutting point (Xp,Yp) for every orientation value.
J Xp Yp
0
1
2
3
4
5
6
7
8 Xs
Xs+R
Xs−R
Xs−R
Xs+R
Xs+R
Xs
Xs−R
Xs
Ys
Ys+R
Ys+R
Ys−R
Ys−R
Ys
Ys+R
Ys
Ys−R
The tool path correction works according to the intersection point
procedure. If the profile transition angle is wide, the intersection point can
be located very far from the path. In this case, linear intermediate blocks (L0,
profile transition angle > 270 degrees) or a circular transition (L1, profile
transfer angle > 180 degrees) are generated. The compensation is switched
off by G40. Changing from G41 <−> G42 without intermediate G40 is
allowed.
N100 G41 R1 Tool radius correction with 1 mm tool radius "on".
N110 G1 X10 Approach block
N120 G1 X20 Y10 First profile block
Syntax
Meaning of the addresses
Explanation
Example