Hi, hope you fine gentelmen can help me. I'm trying to get a acroloc series 10 with a fanuc 6m control working but I am having trouble with setting the part zero and tool length offsets.

The procedure I plan on using is:
I want to use a G54 x y and z in my program.
Setting the G54 from my programmed part zero.
Setting the G54 Z from the top of my part.
Setting the tools from the machine table using a 1" block.


1) I fire up the machine and home out x,y and z axis.
2) I then go to each position page and hit x origin,y origin and z origin.

FROM here I am LOST!

PLEASE, if someone could fill in the blanks for me!

3) I move the x and y axis to my part zero, now what page do I enter the
values for my G54 offset?
4) How do I set the G54 Z axis offset?
5) How do I set the tool ofsets?

I just tonight figured out how to enter a tool offset, I have to enter (hit) the p key first then the z value at the bottom of the screen, but the tool does not go anywhere it is programmed to go.

I have many years experience but this control is something else.
My patience with this machine is very low, I'm working a 12 hour shift at my day job and trying to help a friend out making some parts that are due Monday with this machine. I'm hoping someone or several of you can help me out.

Bless you if you can and THANK YOU!
Tom

Hi Tom,

Its a very old one, i'm not sure if there is a G54 in it. It could have be an option in those days.

What you can do, first go to zero return position, and than put in your program someting like
G92 X100. Y-100. Z-100
G00 G90 X0. Y0. Z0.
You will see the axes moving to your G92 position.
This will shift your coordinate system to X100. Y-100. Z-100.

Finish the program with G91 G28 X0. Y0. Z0. The axis move to machine zero position, en then G90 G92 X0. Y0. X0. This will shift your coordinate system back.
Try to play with this a little, you will find out soon:D

Take a look here: http://www.cncezpro.com/g92m.cfm

Good luck!

Thank You for the reply. The machine/control accepts a G54, their is a program that is in the machine that was written by a technition to do a couple tool changes and some machine movement. It has a G54 command to go to after each tool change, the machine performs that command in the program but:
I'm using that program while changing offsets, G54 and tool offsets, to try and figure out where the machine goes to after making the offset changes, but i still can't come up with the proper sequence.
For instance, after finding my part zero do I go to the offset page that lists six different machine offsets and type in the machines absolute value, hit x origin, y origin and do I need a G54 Z or does the program get it's z value from the tool offsets and the origin I set after homing the Z axis after firing it up.
I hope I understand your reply, I've used G92 in the ast but it's been awhile.
Tom

Set the tool lenght on the top of the part, leaving the G54 z value at zero, I think you'll have better luck. This how we run ours.

Thank you I'll give that a try.

You wrote, you fill in the absolute position in the G54 offset.
This is where it goes wrong, you have to fill in the 'machine' position.
You don't have to hit x, y, or z origin. This wil set your relative coordinate system and i don't think you use that one.

The z axis zero position can you do in a simple way, just touch with a tool that has an offset of "0" (callibration tool) the top of the product, and fill the 'machine' position in the G54.
The other tools will now have offsets that are the difference between the callibration tools and the new tools.

Again, good luck!

thank you hangslot,
I think I gathered some good ideas and tommorrow evening I
will try them each one at a time in a hopes I can understand
what this control needs to run as I expect it to.
I will report my findings as soon as I can.
Thanks to all!
Tom

1st when you turn your machine on, and zero return your machine to machine home
only origin the display without the dots under X Y Z. this is the relative position page.
the [page down] position page with dots is absolute position which is automaticly changed iwth ZERO RETURN or G54,G55,etc. After finding part X0,Y0 write down the values from the relative position page(the one without dots), and inter them into the G54,G55,etc. offset. then press RESET the the absolute page (with dots) should change to X0,Y0.

Z value is the differance between where you set your tools and part program Z zero

Thank You Cad, I got it working but your post helps alot.
In short I homed machine, found the relative position page
and hit x origin y origin and z origin.
Edge found my part zero, went to the absolute page and
again went x origin, y origin.
Loaded my longest tool in the spindle, touched off the top of
part, (z0), went to the machine offsets, g54, offset 01, typed in
z0 input.
tool offset page cursor down to the tool # and hit, z input.

Machine is a dinosaur and an accident waiting to happen, now
I have to figure out how to get a part program from mastercam
to the controller so I dom't have to type in each program.
Thanks Everyone!
TC