Reading The Current Nc Information - HEIDENHAIN CNC PILOT 640 User Manual

4

Reading the current NC information

Use the following syntax to read NC information that was
programmed with G codes.
Identification codes for NC information
#n0(X) Last programmed position X
#n0(Y) Last programmed position Y
#n0(Z) Last programmed position Z
#n0(A) Last programmed position A
#n0(B) Last programmed position B
#n0(C)
Last programmed position C
#n0(U)
Last programmed position U
#n0(V) Last programmed position V
#n0(W) Last programmed position W
#n0(CW) Tool insert angle (0 or 180 degrees)
#n18(G) Active working plane
#n40(G) Status of TRC
#n47(P) Current safety clearance
#n52(G) Oversize G52_Geo taken into account 0=no / 1=yes
#n57(X) Oversize in X
#n57(Z) Oversize in Z
#n58(P) Equidistant oversize
#n95(G)
Programmed feed type(G93/G94/G95)
#n95(Q)
Spindle number of the last programmed feed rate
#n95(F) Last programmed feed rate
#n97(G) Programmed speed type (G96/G97)
#n97(Q) Spindle number of the last programmed speed type
#n97(S) Last programmed speed
#n120(X) Reference diameter X for calculating CY
#n147(I) Current safety clearance in working plane
#n147(K) Current safety clearance in infeed direction
Access to current NC information
#nx(select) x = G-code number
select = designates the information to be
read
Active working plane
#n18(G) 17: XY plane (front or rear)
18: XZ plane (turning)
19: YZ plane (plan view / lateral surface)
468
DIN/ISO programming | Programming variables
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017