Need Help!- Hwacheon HiEco31A w/Fanuc 18T

[PDI-Curtis]

We recently purchased a Hwacheon HiEco31A with a Fanuc 18T control. I have been having some trouble getting it to operate in the same way as our Daewoo Puma 200 with the same control. I am using G50 to establish my work shift... this works flawlessly on the Daewoo:

N5 G50 X10. Z8. M41
G0 G97 S313 T0500 M3
X4. Z1. T0505 M8
X0
Z.1
G1 Z-.3 F.003
Z-7.7796 F.007
G0 Z.1 M9
X4.
X10. Z8. T0500 M5
M30
%

When the Hwacheon goes home (the line above M30), it takes off in the wrong direction. Is seems to be that it is not cancelling the geometry offsets as it goes home.

Is there a parameter setting that controls how this works? As I mentioned, I can load the same code into the Daewoo and it works fine.

[fordav11]

18 series has geometry offsets and workshifts so you should not need to use G50 X Z

Your issue is a classic misunderstanding of how CNC machines/CNC controllers work and perhaps a lack of updating to current setting methods.... G50's were only used on very early 80's controls and have been totally obsolete for at least 20 years. You have a very nice modern controller and you should use it's power to your advantage.

If you cancel the tool offset (the T0500 near the end) and have a movement command on the same line then the absolute position which was previously based on your work Z0 will change to the machine coordinate system on your display and your tool will appear to move in the wrong direction. that's because S, T and M functions are completed BEFORE any other command on the same line in a program. So tool offset is cancelled first then your tool tries to move to X10. Z8. but there is no valid work coordinate system active so it reverts to machine coordinate system which has no relation to your work Z0.

This is a potentially dangerous crash situation because the machine/controller has no info about where your part and tool is since there is no valid geometry offset. With no valid geometry offset the X and Z will usually both be large negative numbers.

You must keep your work coordinate system (and thus geometry offset) active until you have finished all movement with your current tool and cancel the offset without any movement command on the same line then you can return to the home position using G28.

Try this....

N5 G50 M41
G0 T0505
G97 S313 M3
G0 X4. Z1. M8
X0
Z.1
G1 Z-.3 F.003
Z-7.7796 F.007
G0 Z.1 M9
X4.
Z1.
T0500 M5
G28 U0 W0
M30
%


you will also need to set your workshift Z0 (G54 in workshift page) using your workshift setting tool and tool 5 geometry will also need to be set correctly. correct operation of your machine may also include re-setting all of your tools the right way to current standards.

[PDI-Curtis]

Thanks for the advice. I'll toy around with it some and see what I can get resolved. I still don't understand why it works fine on our Daewoo w/Fanuc 18T though.

Part of the reason we program that way is because we have older machines that DO need the G50 method, and in the interest of keeping everything programmed in roughly the same method, we have done the same with the 18T controls.

[fordav11]

thats kind of like buying a Ferrari and driving at 10mph because they used to drive at that speed in 1920
you should update your methods and make the machine do the work. the setting time will also be GREATLY reduced and your life at work will be generally easier

someone should do a poll to see if anyone with later controls uses G50's. I doubt anyone else on Earth does