G54 TO G59

[Stebedeff]

Hello to all,

Is there any way to have more workoffstes then just the G54 to G59?
Suppose I need to clamp 20 parts. How could I have 20 workoffsets?
If I had to do this rightaway I guess I would use the G92 code. But I'am still curious of other methods. Does anyone have any better ideas?

Greetings...

[beege]

There's a G54.1 option, which gives you 48 more. Or you could use the G10 data setting option to change the values from within the program. Unlimited that way.

[psychomill]

or you can get G54.1 and get 300 more (next option above the 48)...

[Andre' B]

I have always found it easier to skip the G10 stuff and just go direct to the variables that hold the offset values, you do need the macro B option but in my opinion a CNC without macro B is crippled anyway.

#5221=-11.6788(G54 X-AXIS) 
#5222=-3.9002(G54 Y-AXIS)
#5223=-13.1752(G54 Z-AXIS) 

#5241=-11.6788(G55 X-AXIS) 
#5242=-15.1141(G55 Y-AXIS) 
#5243=-8.1257(G55 Z-AXIS)

#5261=-36.967(G56 X-AXIS)
#5262=-5.500(G56 Y-AXIS) 
#5263=-19.1192(G56 Z-AXIS) 

#5281=-36.967(G57 X-AXIS)
#5282=-5.500(G57 Y-AXIS) 
#5283=-19.1192(G57 Z-AXIS) 

#5301=-36.967(G58 X-AXIS)
#5302=-5.500(G58 Y-AXIS) 
#5303=-19.1192(G58 Z-AXIS) 

#5321=-36.967(G59 X-AXIS)
#5322=-5.500(G59 Y-AXIS) 
#5323=-19.1192(G59 Z-AXIS)

[psychomill]

Andre... I think you missed Beege's point about the G10 use....

and although I agree about Macro B... I don't see how you think this:
#5221=-11.6788(G54 X-AXIS)
#5222=-3.9002(G54 Y-AXIS)
#5223=-13.1752(G54 Z-AXIS)

.. is easier to use than this:
G10L2P1X-11.6788Y-3.9002Z-13.1752

... for the purpose of the thread topic...

[stevo1]

What kind of Fanuc control are you using?? I assume that you already have the G54-G59 workoffsets? You just need to get the extended offset option turned on. If not...I agree that using the G10 data setting is the easier route to go.

Depending on how you are locating the parts, if your using any kind of probing or there is any relative number from 1pc to the next you could go many ways in setting up variables and calling them using the G10 setting.

If you have or use macro programs you would use a macro modal call that will call the program specified and when it returns it reads your next coordinate(part placement) and reruns the program to the next part. If your 20 parts are always in the same placements you could just use a maco call instead of a modal call.

Your options are almost limitless when it comes to macros, but I don't want to ramble to far OT from the original question.

Stevo

[Geof]

Originally Posted by psychomill Andre... I think you missed Beege's point about the G10 use.... and although I agree about Macro B... I don't see how you think this: #5221=-11.6788(G54 X-AXIS) #5222=-3.9002(G54 Y-AXIS) #5223=-13.1752(G54 Z-AXIS) .. is easier to use than this: G10L2P1X-11.6788Y-3.9002Z-13.1752 ... for the purpose of the thread topic...

Even easier; four fewer characters to type.

G52X-11.6788Y-3.9002Z-13.1752

[psychomill]

... for the battle of the keystrokes...

All right Geof, you win ....

But G52/92 opens up a different can of worms and we've all been in there before on other threads... However it still qualifies as a method... For note, Andre's does too. It's just a boat load of writing for what's taking place.

[chucker]

This is how I do it if I use G10 operators are not allowed to change program to adjust the g10 this puts offset in variable so they can ajdust it with out editing program you can have as many offsets as you need.

O0900(900 TOPS)
(MAKE 3 PARTS)
(3.25 IN STICK OUT)
(#555 IS Z WORK OFFSET)
(#555=3.6582)
N100T707(BORE FOR 3 PARTS)
#5242=#555 takes the number from #555 and puts it in g55 Z offset)
G52Z0(TRUE G55) then use this to shift for next part
G55
G99
G50S2000
G96S1200M4
G0X2.5Z.2M8
G1Z-2.95F.014
X2.45
G0Z1.M9
X8.Z2.
#507=#507+1 (counts parts on insert)
IF[#507GE#607]GOTO1000
IF[#507LT#607]GOTO1001
N1000
#507=0
#3006=1(CHANGE BORING INSERT)
N1001
M1

other tools here


N210(ROUGH 2ND PART)
#5242=#555
G52Z0(TRUE G55)
G52Z-.98(G55 SHIFTED MINUS .980)next part shifted
T101(CNMG 432 FACE TOOL)
G99
G50S2000
G96S1800M4
G0X4.2Z.01M8
G1X3.1F.014
X2.1F.006
G0X4.2Z.05
Z-.122
G1X3.025F.014
G0X3.885Z-.1
G1Z-.362
X4.2
G0X8.Z6.
#501=#501+1
IF[#501GE#601]GOTO5000
IF[#501LT#601]GOTO5001
N5000
#501=0
#3006=5(CHANGE ROUGH INSERT)
N5001
M1