[Barney]

I need to know how to do this on a Fanuc mill controller, please let me know how to do it, thanks.

[Ozemale6t9]

I have explained this once before in this thread: http://www.cnczone.com/forums/showpo...52&postcount=2

regards, Oz

[vpcnc]

G54 to G59 are a Fanuc Option.
If your Machine Builder didn't supply them you will need to conact the builder, dealer, or Fanuc to purchase the option.

[dlokon]

Fixture offsets (G54 thru G59) are NOT an option - they're standard.

[Barney]

I was reading the manual from my machine and found out that you can also set a fixture offset called G54.1 P(n) and set up to 48 different locations, pretty nice information. That means you can set all of these different fixture offsets in "addition" to the the usual G54 thru G59 we were discussing earlier. My question about how to set the fixture offsets earlier was specifically if there was a button you could push to quickly insert* the value of the axis location into the XY or Z G54 value location? I found out there is not, you have to enter the Absolute value of the axis location into the field manually. If you need more information about how to set and enter the G54.1 P1 thru P48 values email me or post to this forum and I will try to assist you. I want to thank you all for your help, yesterday I was able to complete the two pallets on my NTC Flexible Vertical CNC machine and write programs to machine the two pallets for a job. This was a recent purchase and I was not familiar with Fanuc mill controls at all. I have been running Fanuc cnc lathe controls since 1994 and had formal training in Chicago at Daewoo tech center, but had not had any training on the details of mill (0-M or 21M) controls. The NTC (Nippei Toyama Corp of Japan) is a really nice machine, pallet is similar to a Daewoo VMC-40, machine is running and ready to make parts later this week, thanks again for your help on my problem. Barney:cheers:

[dcoupar]

Barney,

I may be all wet, but you might try this:

Bring your .200 edge finder up to the left hand (X-) edge of the part, then retract Z.

Go to the Work Offset page, then cursor to the offset # you want to set (or type in the offset number, and press the [NO.SRH] soft key). You don't have to be in the X field, just in the correct offset #.

Type X-.1, then press the [MEASUR] soft key. If you don't see the [MEASUR] soft key, then your machine may not have the option (I believe it's called Direct Input of Offset)

Good luck.

Dave

[dlokon]

Barney -
There are 6 standard fixture offsets on every Fanuc control - G54 thru G59. The additional fixture offsets G54.1 P1 thru G54.1 P48 are usually optional.
I was a CNC Applications Engineer from 1985 thru 2000, when I had to retire due to health reasons. I do, however, still teach CNC programming. Prior to going into CNC applications, I spent 15 years as a machinist.

[Barney]

Thanks, I guess my machine has them because it works on my 21M Fanuc control, I thought they might be in all the machines, anyway have a happy new year. Barney

[jamesweed]

If macro enabled, you can use simple macros to automate some of these actions. Here is a example macro that sets work coord in G54...

%
O0002(SET WORK COORD. G54);
#3003=1;
IF[#24NE0]GOTO1;
#5221=#5021(X AXIS);
#33=0;
N1IF[#26NE0]GOTO2;
#5223=#5023(Z AXIS);
#33=2;
N2IF[#1NE0]GOTO3;
#5224=#5024(A AXIS);
#33=3;
N3IF[#33NE#0]GOTO4;
#5221=#5021;
#5223=#5023;
#5224=#5024;
N4G54;
#3003=0;
M99;
%

This can be called in a program or MDI like so...
G65P2; ( no arguments sets all three axis's to zero XZA) or you can set one or more at a time using arguments) like this G65P2X0Z0
This macro could be altered to set different axis's. Way easier then going to work coord screen and using measure funtion. Macros are real time savers.

[vpcnc]

I wanted to clarify something that was posted a few posts back.
For as long as I've worked with Fanuc controls (some 23 years) I've never known anything to be "STANDARD"
Every Control that I've had to Build, I've had to order every feature I wanted from a list of options.

When a machine tool builder picks out a control Package, they too have to select all of the Fanuc options that they will include with the package.

Perhaps a machine tool builder will list a Feature as Standard simply because they have included it with the price of the machine.

However, there are Machining Centers that came without the Fanuc Work Coordinate System. It was an Option. A02B-0099-J830 for the 0MC, 0MF,0MD series of controls.

I've attached a sample Fanuc Data sheet which shows the options selected for that particular build of control.
In the List you will see the option called Work Coordinate System listed.

[vpcnc]

Here is an Excel Document that I put together.
I hope some of you will find the information helpfull.

Depending on What Work Offset Option you have.
G54-G59
The Extended 48
or the Extended 300

Tool Offsets could be Offset A, B or C type offsets.

The Variables used to Access them and the work offsets will be different from one Option level to the Next.

I've tried to Show all the Different Variables with the different levels of Work and tool Offsets.

The Excel document has three sets of Tabs or Three worksheets along the bottom. Be sure to View Each Sheet.

As a Macro Developer, one has to be Careful to know excatly what options the particular Machine has for Work Offsets and tool Offsets.
Otherwise you Might end up working with the wrong Variables.

[bbyelme]

Hi
In Fanuc you can use common offset as a primary and all other work offsets G54 to G59
G10G90L2P0 X Y Z for common (make sure after use end with G10G90L2P0 X0 Y0 Z0 to make it zero)
G10G90L2P1 X Y Z for G54
P2 for G55
P3 for G56 and so on
If you want to use offset on offset use Macro for calculation

[cmoretti1979]

If macro enabled, you can use simple macros to automate some of these actions. Here is a example macro that sets work coord in G54...

%
O0002(SET WORK COORD. G54);
#3003=1;
IF[#24NE0]GOTO1;
#5221=#5021(X AXIS);
#33=0;
N1IF[#26NE0]GOTO2;
#5223=#5023(Z AXIS);
#33=2;
N2IF[#1NE0]GOTO3;
#5224=#5024(A AXIS);
#33=3;
N3IF[#33NE#0]GOTO4;
#5221=#5021;
#5223=#5023;
#5224=#5024;
N4G54;
#3003=0;
M99;
%

This can be called in a program or MDI like so...
G65P2; ( no arguments sets all three axis's to zero XZA) or you can set one or more at a time using arguments) like this G65P2X0Z0
This macro could be altered to set different axis's. Way easier then going to work coord screen and using measure funtion. Macros are real time savers.

I noticed that A axis is coded but shows no Y axis.
What is the difference?