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
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)
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.
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 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.