Hi i have a simple Programm:

running on Mach3
tested in R3.043.022
and in R3.043.066

N1 ( Lochreihe mit: 2 Loecher)
N2 ( Zentrierbohren mit Werkzeug: 99 )
N3 ( Bohren mit Werkzeug: 114 )
N4 G00 G49 G40 G21 G17 G80 G50 G90
N5 ( Zenrierbohren ----------)
N6 M06 T99
N7 G90 G00 X5 Y10
N8 G00 Z5
N9 S3800
N10 M03
N11 M08
N12 G73 X5 Y10 Z-3 Q1 R5 F300
N13 G91 X7.0711 Y7.0711 L1
N14 G80
N15 G90
N16 G00 Z5
N17 M09
N18 M05
N19 ( Bohren ----------)
N20 M06 T114
N21 G90 G00 X5 Y10
N22 G00 Z5
N23 S1100
N24 M03
N25 M08
N26 G73 X5 Y10 Z-20 Q1 R5 F230
N27 G91 X7.0711 Y7.0711 L1
N28 G80
N29 G90
N30 G00 Z5
N31 M09
N32 M05
N33 M06 T0
N34 M30

if i run the line:

N7 G90 G00 X5 Y10

i get a random z-axis movement

at line:

N21 G90 G00 X5 Y10

witch is exactly the same i have no z-axis movement

if i Switch the lines:

N7 G90 G00 X5 Y10
N8 G00 Z5

to

N7 G90 G00 Z5
N8 G00 X5 Y10

everthing works like expected.

i have no real idea who or what initiates this z-axis monent.

TPS

So,
after hours of fiddeling and testing, i found the Problem.

my TC macro (M6Start) was based on an example from CSMIO.

at the end of the macro was the following code to anunce the new tool to the System:

  SetCurrentTool( newtool )
  Code("G43T" & newtool)
  Code("G43H" & newtool)

i never thought about it

but the G43T.. caused the Problem.

so i started to get informations what G43T.. exactly does (or should do),
without any success.

so it is running now without this G43T..,and without knowing what is should do.
i can live with this.

TPS
 
 

G43 Htt is calling the tool offset for the current tool, if all your offsets are zero then nothing happens.

For example G43 H4, tool offset 4 has a length offset of 10mm then when the machine moves even without a Z move commanded the tool is moved to allow for the offset.  G43 T4 will do the same but will assume H4 unless commanded otherwise.