coordinate system shift

[elraiis]

hi guys... simple and quick thing for sure for those who used this before... am always working with machines that has around 40 to 50 G's... few weeks ago we got a machine that has only G54 TO G59 and its not enough for production at all... so i want to be sure if anyone can help if i use the G10 L2 G54 X_ Y_ WOULD THAT SOLVE IT? AND I CANCELL the command by G11?

 

meaning if i'm to say my G54 is X1 Y1 Z0. AND MY SECOND PART IS LOCATED 5 inches away ON X AXIS so is this going to be correct:

G10 L2 G54 X5.0Y0.0

PROGRAM

G11

?????

thanks in advance for any avalable help. This machine is 2 pallets 40x20 each and 6 offsets is no enough...

 

and a good morning to all

peace

[Bruce Caulley]

One way around this is to call your offsets with a sub. In the sub you have for example G92 XYZ

 

At the top of the programme you call that sub and then your datum is set. This way you can have your offsets numbered as per job# or QC fixture location.

 

Just one way to do it.

 

Bruce

[d.park1]

Sometimes machines with only G54-G59 can also use G54.2-G54.9 all the way thru G59.2 etc.

[Dave Ball]

To answer your question, yes. I have used G10 to reassign my work offset as I progress through a program, just be sure to keep up with which one is active and document things very well so others will understand what is going on. By the way, using G10 to set values is an OPTION on some controls, are you sure yours is turned on?

[DavidB]

G10= Data Input

L2= Workoffsets

P1= G54, P2=G55 and so on.

 

quote:

---

meaning if i'm to say my G54 is X1 Y1 Z0. AND MY SECOND PART IS LOCATED 5 inches away ON X AXIS so is this going to be correct:

G10 L2 G54 X5.0Y0.0

---

You would need

G10 G90 L2 P1 X6.0

The Y and Z will stay modal.

[Dave Ball]

quote:

---

meaning if i'm to say my G54 is X1 Y1 Z0. AND MY SECOND PART IS LOCATED 5 inches away ON X AXIS so is this going to be correct:

G10 L2 G54 X5.0Y0.0

---

code:

---

 G91 G10 L2 P1 X5.0 

---

This will get you from X1.0 to X6.0

Always remember the G10 setting is set in relationship to G90/G91, you can set locations using either absolute or incremental.

 

There is a chance your control has extended offsets, G54.1 thru G54.48, to test this try using G54 P1 thru G54 P48 in place of regular G54 thru G59. If you have these they can also be set in either absolute or incremental using G10 like this for absolute

 

code:

---

 G90 G10 L20 P1 X1.0 Y1.0 Z0 

---

or like this for incremental

 

code:

---

 G91 G10 L20 P1 X5.0 

---

[YoDoug®]

you could use G52

 

G52 G91 X5. Y5. will shift all work offset incrementally

 

G52 G90 X5. Y5. will shift all work offset to absolute postion of current work offset.

 

G52 G90 X0 Y0 will cancel, M30 or reset will also cancel.

[elraiis]

hi guys

OMG thanks alotttt for all the replies. some machines we have have teh G54.1P1 ALL THE WAY UP TO P49 I THINK.. this one doesn't. ShefferCNC thanks for pointing out that the G10 is an option.. i didn't know that i have to check.. and as for the G52! THE MACHINE has no G52! I THINK there is the workshift but whats assigned to it is 00 and no G52.

Thanks for all help i'll try to test tomorrow.. today was one hell of a day i worked a straight 15hrs i need to go rest guys.. good night

and thanks again

[elraiis]

HI GUYS...

ok.. i screwed up somewhere anyone's input is beyond welcome..

G91 G10 L2 P1 X-5.0

 

This shifted my coordinate system and G11 is not cancelling it!!! even after i reset the machine's x axis is shifted! here is what i put and sorry again

 

**********

:0000

( 77054 )

G20

G0 G17 G40 G49 G80 G90

T1 M6

( 1/2 EM )

( FACING ZERO LVL )

G0 G90 G59 X-3.5825 Y-.4974 S8500 M3

G43 H1 Z.3 M8

M98 P0001

( FACING ZERO LVL )

G91 G10 L2 P6 X-4.275

G90 X-3.5825 Y-.4974 Z.3

M98 P0001

( FACING ZERO LVL )

G91 G10 L2 P6 X-4.275

G90 X-3.5825 Y-.4974 Z.3

M98 P0001

G11

( -0.002 DEEP STEP )

G90 G59 X0. Y1.8 Z.3

M98 P0002

( -0.002 DEEP STEP )

G91 G10 L2 P6 X-4.275

G90 X0. Y1.8 Z.3

M98 P0002

( -0.002 DEEP STEP )

G91 G10 L2 P6 X-4.275

G90 X0. Y1.8 Z.3

M98 P0002

G11

( -0.01 DEEP STEP )

G90 G59 X-1.9125 Y.981 Z.25

M98 P0003

( -0.01 DEEP STEP )

G91 G10 L2 P6 X-4.275

G90 X-1.9125 Y.981 Z.25

M98 P0003

( -0.01 DEEP STEP )

G91 G10 L2 P6 X-4.275

G90 X-1.9125 Y.981 Z.25

M98 P0003

G11

( ROUGHING THRU POCKET )

G90 G59 X-1.76 Y.013 Z.3

M98 P0004

( ROUGHING THRU POCKET )

G91 G10 L2 P6 X-4.275

G90 X-1.76 Y.013 Z.3

M98 P0004

( ROUGHING THRU POCKET )

G91 G10 L2 P6 X-4.275

G90 X-1.76 Y.013 Z.3

M98 P0004

G11

M5

G91 G28 Z0. M9

G28 Y0.

M30

*********

am sure i screwed up but i donno where.. anyone can help plz? and say if i use G90 instead of G91 what diff is that going to do

peace

p.s it worked perfect until the first G11 then it kept adding to the X value becuase then my spindle didn't come back to the origin G59 LOCATION but kept going on forward!!!

[Guest]

count how many times you shifted it and go back the other way at the very end of the program.

 

I see 7 shifts

 

code:

---

G91 G10 L2 P6 X-4.275

---

so add

 

G91 G10 L2 P6 X29.925

[elraiis]

But why G11 did nothing? i counted back and shifted 3x4.275 and my x is back to normal.. becuase the part didn't continue beyond the first G11 as i got a over travel.. so? thanks alot for the reply.. but how do i cancel? do i replace my G11 by G91 G10 L2 P1 X{THE TOTAL DISTANCE MOVED THE OPPOSITE DIRECTION).

 

i have 3 identical parts next to each other. so say what i had in mind thru my program is i do face part one, face part 2, face part 3, then pocket part one, then 2, then 3 and so one. it did the first 3 faces but didn't come back to part one no more. i hope that made my situation a little more clear and thanks again man for all and any help.

 

peace

[Dave Ball]

G11 is not necessary to cancel G10. Canceling it does not reset your initial value back to its original value. In fact G11 doesn't show up in most machine manuals. I would suggest that you use G10 G90 at the end of your program to reestablish your original G54. If ya want email me your code and I will fix it for you.

[elraiis]

thanks for the help.. e mail the code? meaning the MC9 file? or that would mean the NC file?

 

thanks

[chris m]

While all of the above suggestions are good ones, and you could probably use G92 as well [which is scary, but would probably help out in some cases] I would suggest calling Fanuc or your local Fanuc hacker and sak them what it would cost to turn on the expanded work offsets. I think it'd be worth it in the long run.

 

C

[Dave Ball]

I don't run MC9 so that file wont be very helpful, but if you send me the NC file I will edit it to work like you want and you can at least see one of the methods. There are many ways to do what you want and not all of them have been mentioned here but chris is right, turning on the extended offsets may be the best long term solution.

[elraiis]

thanks alot guys and sorry for replying so late.. and u nkow what i won't need to go through this headache.. not because of the headache but i feel is 'scary' to shift the coordinate offset back and forth like that. so i mentioned the situation to the boss and its up to him to update the memo of the machine if he intends to keep it that is.. so i took it out of my hand and put it in his.. thanks again and sorry for being a pain in the A$$.