need help, fanuc control

This is the first time on a fanuc mill for setup for me so please don't be to hard on me.
Maybe I am doing this right, maybe not. I have a fanuc 21mb control. I learned to set z and trying to set x,y buy touching off my stock in relitive position ( x-9.,y-5.)- type in y0-preset, x0-preset and this changes my relative position to x0 y0 and can jog back to abs 0 and show that relative is working. When I try to run a program already in the machine, there are g54"s in the program but it seems to want to use ref 0 as it's cordinates.
My rel pos was y-5. and x-9. with g54 in the program go x0,yo, it stays home. Put in x-9.,y-5. and it goes to my 0 point. I am reading the manual trying to figure this out and I think I read g54 is an option? Please tell me that can't be. The control shows all g54-59. Anyway I'll be out in the shop still trying to figure it out but if g54 really is an option I am beating my head against a wall.
Any ideas appreciated.
Daryl

I think if G54-G59 is showing up in the work offset page then it is installed in the machine. Look at G54, are the values in the table the same distance it is off? If not, changing them to zero should fix it.
Dave

Where in michigan are you, I'am in Sarnia Ont. Canada. If you are close I can show you how to do this.

I'm near Cadillac MI 49601
Schneider, Not sure what you mean but with relative x0,y0 (abs@ y-5. x-9.) I go abs x0,y0 relative is at x9.,y5. I also have a relative Z .75 in. I'm not for sure here but when I ref 0( which I don't always do) I think all (rel,abs, and machine) x and y's are 0 with z staying at .75 in rel. Maybe trying to hard and going to fast. Need to take a deep breath and start again.
Daryl

I got it, but it don't seem logical to have to type these positions. You also use relative to set z but not x and y but rather type in all your x and y positions in g54 offset table. I guess I had to type in z values in the offset table last night also. I read here how to mass modify all your tools in z for quick setups. I tried, but got it wrong (z overtravel)
At least I could make some parts, but setup will be slow till I figure out somthing better. Anybody with shortcuts I will be grateful.
Daryl

dandjp:

I can not give you specifics on a Fanuc, but here is some basic theory.

Somewhere there is a machine absolute zero position. On HAAS machines, in many ways similar to Fanuc, the machine absolute zero is with the table fully to the left, and toward you, and the Z is at the tool change position. This means the X Y zero is at the right rear of the table. Thus, the machine has to be at some -X and -Y absolute position to work on a part.

If want a work coordinate system with a 0, 0, 0 position somewhere else than the right rear corner of the table and tool change, then you need to load some non-zero offset values into a G5k offset table, and specify that G5k in your program. Assume the table travel is 30 in X and 16 in Y, then -15.0 in G5k X, and -8.0 in G5k Y will make the G5k zero coordinate at the center of the table. After you specify the G5k in your program, then
G0 X1.0 Y-0.75 will position the table at the absolute position X = -14.0 and Y=-8.75.

Suppose you want the left rear corner of your part to be at 0,0 relative to G54 0, 0, and you use an 0.2" edge finder. The machine absolute X reading is -20.15 when the edge finder has found the edge. You need to put -20.05 in the G54 X location in the OFFSET table, etc.

.

I worked in a tool and die shop for 14 years (14 on cnc lathe and the last 4, mostly cnc mill. I never saw anybody including me ever type in a g54 reference # nor did we ever type in a length offset. We ran Haas and Fadal.

Fanuc work offsets.

Here is how you can do it on every Fanuc mill control since the 6M.
Do a Zero return.
Clear out the Relative X and Y to read Zeros.
Then Jog or use the Handwheel to pick up the lower left corner of your part with a wiggler(or wherever you want to measure from).
Write the dimensions that you travelled from Home down.
Go to G54 in the Offset screen and put the distance from Home into the X and Y of the G54.
To test it, write a little program and run it in single block from Home after you do a Zero return.
O1000
G90 G54 X0 Y0
M30
When you get to X0 Y0, stop and crank it down and check if you are really there.
Its very easy once you know it, if you still have questions, call me tomorrow at 614-888-8466.
Heinz.
http://home.columbus.rr.com/hputz





Heinz.
http://home.columbus.rr.com/hputz

When setting positions, go the the work shift (G54....) page and set to 0 when setting X,Y,Z. Depending on the options you may set X,Y,Z to the number you see in the positions for each. Call G54,G55...and so on in your program for each you set. Tis the same thing as E1,E2,...in your Fadal. Just as part location E1 may be the first vise and retain the X,Y,Z you still need to call H for tool height (and D id your are using G41&G42) for each Txxxx you use. G54 (E1) may be used for every tool just like Fadal. G55 (E2) is the next vice and so on...I'm sure you get it.

Dang it...walked away mid-type, and came back to finish and submit, and I see Heinz has done a much better job of explanation than I. It's obvous he (Heinz) is meant to teach.

Yes THANK you guys . That is what I did, but would like a better way than typing those #s in as dislexia somtimes sets in, and that can be a real problem on the 2nd op.
Again thanks so much. This is a good forum and may become invaluable.
Daryl

dandjp:

A correction to my previous post relative to HAAS. What is displayed on the offset page are positive values of the machine absolute position where your G5k origin is located.

To continue from my previous post. On a HAAS machine there are at least four ways to set or load values into the offset table.

1. Manually load the value. You select the OFFSET page, move the cursor to the location to change, type the desired value, and press F1 to write the value into HAAS memory.

2. Simple load method. Move the table to the desired XY location. Select OFFSET page, move the cursor to the location to change (X first), press the PART ZERO SET key, the cursor automatically moves to the Y position, press the PART ZERO SET key again. The automatic cursor move is not useful when using a 0.2" edge finder because you need to apply an 0.1 change to the loaded offset value.

3. G10 means. Use the G10 function from a program or MDI to load the desired location. With MACROS you can get the current machine position and load this into the desired offset location with G10.

4. Direct addressing method. #5221 is the variable address for G54 X, and #5222 for G54 Y. #5021 is the machine current absolute X position.

From within a program or MDI you can do
#5221 = 15.0 (to load 15.0 into G54 X.)

If you use a pointy tool for locating your G54 X0 Y0 position, then executing the following program would automatically load the G54 X Y table locations with the current machine absolute location.
%
O8000
#5221 = #5021
#5222 = #5022
%
Whether you use -#5201 or #5201 will depend upon on the year of the HAAS machine.

If you use a 0.2" edge finder, then you need four programs.
%
O8000 (X set of G54 for 0.2" on left side)
#5221 = #5021 - 0.1
%

%
O8002 (X set of G54 for 0.2" on right side)
#5221 = #5021 + 0.1
%

etc.

There may be some sign problems. You have to verify this for a particular machine.

You can also use RS232 to load the OFFSET table.

.