Reading The Current Nc Information - HEIDENHAIN MANUALPLUS 620 User Manual

Identification codes for tool information
#wn(AW) 0: No driven tool
1: Driven tool
#wn(MD) Direction of rotation:
3: M3
4: M4

Reading the current NC information

Use the following syntax to read NC information that was
programmed with G functions.
Identification codes for NC information
#n0(X) Last programmed position X
#n0(Y) Last programmed position Y
#n0(Z) Last programmed position Z
#n0(C) Last programmed position C
#n40(G) Status of TRC (see table at right)
#n148(O) Active wear compensation (see table at right)
#n18(G) Active working plane (see table at right)
#n120(X) Reference diameter X for calculating CY
#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
#n150(X) Cutting width shifted in X by G150/G151
#n150(Z) Cutting width shifted in Z by G150/G151
#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
#n47(P) Current safety clearance
#n147(I) Current safety clearance in working plane
#n147(K) Current safety clearance in infeed direction
358
Access to current NC information
Syntax: #nx(select)
x = G function number
select = designates the information
to be read
Status of TRC
#n40(G) TRC/MCRC status:
40: G40 active
41: G41 active
42: G42 active
Active wear compensation
#n148(O) Active wear compensation (G148):
0: DX, DZ
1: DS, DZ
2: DX, DS
Active working plane
#n18(G) Active working plane:
17: XY plane (front or rear)
18: XZ plane (turning)
19: YZ plane (side view / surface)
ISO Programming