Need Help!- Tool offset problem when running

[lifestill]

Below a short of the G-Code running. The tool offsets work perfect and as they should. My problem is when the program first starts or calls for a tool change.

This happens on every run. Not sure if H can come before T, but that does the opposite. Line 1400 calls for a tool change after the z is moved up 7" inches. When I hit conitinue, the head moves down at homing speed to a point below the material. I have to stop it before ruining the part. If I move the H before T, the tool moves up to 4.10" inches at homing speed before starting the next operation.

Why is the software moving the tool at homing speed at all? It should just set the offset and continue with the new offset. This is just an example, but this happens all the time. I don't see the problem. HELP!!

%
O0000
N90 G49
N100 G17 G40
N110 G49
N120 G17 G40
N130 G20
N140 G80
N150 G90
N160 G98
N170 (.5 HSS CENTER DRILL)
N180 T101 M06
N190 M03 S2291
N200 M08
N210 G43 H101 D101
N220 G00 X0.15 Y5.85 Z2.
N1340 G01 Z-0.05
N1360 G00 Z7
N1370 M09
N1380 (END TOOL)
N1390 (#19 DRILL FOR 5 X .8MM TAP)
N1400 T200 M06
N1410 M03 S6000
N1420 M08
N1430 G43 H200 D200
N1440 G00 X0.15 Y5.85 Z2.
N1450 Z0.05
N1460 G01 Z-0.5499 F5.0 S6000
N1470 G00 Z0.05
N1480 Z2.
N2590 M09
N2600 (END TOOL)
N2610 M5
N2620 M09
N2630 M25
N2640 M30
%

[Torsten]

Try these changes and see if it works for you.

%
O0000
N90 G49
N100 G17 G40
N110 G49
N120 G17 G40
N130 G20
N140 G80
N150 G90 G00 (<- May need this?)
N160 G98
N170 (.5 HSS CENTER DRILL)
N180 T101 M06
N190 M03 S2291
N200 M08
N210 G43 H101 D101 Z2. (<- Moved Z Axes call)
N220 G00 X0.15 Y5.85 (<- Z moved from here)
N1340 G01 Z-0.05
N1360 G00 Z7
N1370 M09
N1380 (END TOOL)
N1390 (#19 DRILL FOR 5 X .8MM TAP)
N1400 T200 M06
N1410 M03 S6000
N1420 M08
N1430 G43 H200 D200 Z2. (<- Moved Z Axes call)
N1440 G00 X0.15 Y5.85 (<- Z moved from here)
N1450 Z0.05
N1460 G01 Z-0.5499 F5.0 S6000
N1470 G00 Z0.05
N1480 Z2.
N2590 M09
N2600 (END TOOL)
N2610 M5
N2620 M09
N2630 M25
N2640 M30
%

[lifestill]

That didn't help The strange thing too is that it always want to go to 4.10".

[Torsten]

Seams you are having a large Toollength in your offfset register.
What methode do you use for setting lengthoffset?
Fanuc's do not work well with large Offsets because of the way Lengthoffsets are aplied by actually moving the tool.
Best to use a Standard Tool or just use the first Tool and set the G54 Offset register based on that.
Other then that you could retrackt the Tool all the way back to machine zero at the end of the sequence as in the example below.

%
O0000
N90 G00 G91 G28 Z0. (<-Retract to Z Machine Zero)
N100 G17 G40
N110 G49
N120 G17 G40
N130 G20
N140 G80
N150 G90
N160 G98
N170 (.5 HSS CENTER DRILL)
N180 T101 M06
N190 M03 S2291
N200 M08
N210 G43 H101 D101 Z2. (<- Moved Z Axes call)
N220 G00 X0.15 Y5.85 (<- Z moved from here)
N1340 G01 Z-0.05
N1360 G00 Z7
N1362 G91 G28 Z0. (<-Retract to Z Machine Zero)
N1370 M09 G90 (<-Add G90)
N1380 (END TOOL)
N1390 (#19 DRILL FOR 5 X .8MM TAP)
N1400 T200 M06
N1410 M03 S6000
N1420 M08
N1430 G43 H200 D200 Z2. (<- Moved Z Axes call)
N1440 G00 X0.15 Y5.85 (<- Z moved from here)
N1450 Z0.05
N1460 G01 Z-0.5499 F5.0 S6000
N1470 G00 Z0.05
N1480 Z2.
N1482 G91 G28 Z0. (<-Retract to Z Machine Zero)
N2590 M09 G90 (<-Add G90)
N2600 (END TOOL)
N2610 M5
N2620 M09
N2630 M25
N2640 M30
%

[lifestill]

I figured it out.

After looking at the M6 macro, I noticed that it was moving the z axis if the position changed during a tool change and that option was turned on. Not sure why it was moving since I wasn't moving anything, but turning that off fixed the problem.

Thanks for input.