NCT Group 99M, 2000M manual Programming Vector Hold G38, Programming Corner Arcs G39

14 The Tool Compensation

14.5.5 Programming Vector Hold (G38)

Under the action of command G38 v

the control will hold the last compensation vector between the previous interpolation and G38 block in offset mode, and will implement it at the end of G38 block irrespective of the transition between the G38 block and the next one. Code G38 is a single-shot one, i.e., it will not be modal.

G38 has to be programmed over again if the vector is to be held in several consecutive blocks.

G38 can be programmed in state G00 or G01 only, i.e., the vector-hold block must be invariably a linear interpolation, or else the control will return error message 3040 G38 NOT IN G0, G1. Unless code G38 is used in offset mode (G41, G42), the control will return error message 3039 G38 CODE IN G40.

An example of using G38:

...G17 G41 G91...

N110 G1 X60 Y60

N120 G38 X90 Y-40

N130 X20 Y70

N140 X60

...

Fig. 14.5.5-1

To program a recession without canceling the offset mode:

...G17 G42 G91...

N110 G1 X40

N120 G38 X50

N130 G38 Y70

N140 G38 Y-70

N150 X60

...

Fig. 14.5.5-2

14.5.6 Programming Corner Arcs (G39)

By programming G39 (I J K),

it will be possible - in offset mode - to avoid the automatic intersection-point computation or the insertion of linear sections when going around outside corners, instead the tool center will travel along a circular arc equal to the tool radius.

It will insert an arc equal to the tool radius in direction G02 or G03 in state G41 or G42, respectively.

99