[FrankCNC]

Hi,

I'd like to use G43, G44 Tool Length Offsets for tools in a Right Angle Head working on the G18 and G19 Planes, the machine ia a Daewoo ACE-H100 with Fanuc 15MA Control. I've tried using...

G43 Z**** H**** (Gauge length of angle head)
G43 X**** H**** (Length of tool in angle head)

but the machine keeps offsetting the Z axis only.
The Programming manual states use G43/G44 Axis**** H**** where (Axis can be any Axis), and also states multiple Axes can also be Offset at the same time using...
G43 Z**** H****
G43 W**** H****
The Machine Tool Reseller Technicians say that the H**** defaults to the Z Axis only but this is different to what the manual says.
Just wondering if anyone has any experience with this issue.

Thanks.

[Superman]

I may be incorrect....but found this link
Fanuc.. G43, G18 fight each other.

which points me to think the format is
G17 G43 Z**** H**** (Gauge length of angle head) ...cutter comp works in the XY plane
G18 G43 Y**** H**** (Gauge length of angle head) ...cutter comp works in the XZ plane
G19 G43 X**** H**** (Length of tool in angle head) ...cutter comp works in the YZ plane
then state again the desired G17/G18/G19....... for the running of the program for arc interpolations correctly
cutter comp works only in one plane, the other axis is to control depth.


If your tool is NOT parallel to an axis, then all three lines would be needed to define the tool tip position relative to the gauge point on the spindle. Cutter comp would not be usable in this instance.
NOTE.... see the link for adding safety lines in your program

[FrankCNC]

Thanks heaps for the link and suggestions very informative

The format you suggested didn't work, still only offsets the Z multiple times, unfortunately the 15M we have doesn't have the 6000 parameter which the link you gave said was for setting Tool Length Comp on any Axis for the 15M, our 6000 parameters only start at 6010 so I'll look into how to add these parameters to or machine.

Thanks for your help.

[norbert.barnard]

Hi,
when all fails, G10 or macroB can work around your situation.

i am using the following method for angular heads.

when mounting the angular head, write the Z + X or Y changes to G54-external (00), with G10 instruction.
X or Y depends on which way the head is facing,
when finnished, write zero to these registers, back to normal.
with this method i don't touch the original G54 (01) set-up.

you need to establish the following dimentions about the angle head:
Z-distance from main-spindle-nose to horizontal center-line of the angle head, (vertical distance = Z)
horisontal distance from the main-spindle center-line to to the right-angle-head spindle-nose face. (horisontal distance = X/Y)

in your situation, you can add the tool length to the X or Y axis value directly ( or using macro registers),
using macro registers you need macro B for this last part.

regards