Hello Guest it is October 25, 2021, 01:25:31 AM

Author Topic: G54 offsets questions  (Read 5732 times)

0 Members and 1 Guest are viewing this topic.

G54 offsets questions
« on: August 10, 2006, 04:22:02 PM »
Hi guys,

This is a copy and paste I did over on cnczone. I wanted to post it here as well since Mach users will understand the software better.

"Hey guys,

There was a thread a few days back that asked about G92 and immediately the thread went to why it shouldn't be used and the G54 up codes should be used instead. I have used the G92 for three years now but see an immediate need to move on. I'm gonna need some help on this.

Let me set the stage. I do not have an industrial strength machine, but it is all I have presently. I use Mach2/3 for my controller and it basically supports all the offset codes. I have a 4th axis that runs parallel to my x axis and I have to be dead centered over the a axis center or my parts are trash. Here's the problem. I use limit switches to set my home positions and for the most part they are within about .005" which is close enough. You will notice I said " for the most part"! My y axis seems to move from time to time and this is the axis that has to be centered over the a axis centerline. I have a known distance from the faceplate of the a axis in the x, which the tolerence really doesn't matter as long as the machine returns to 0 each time after the initial reference move. So far that is the case. Z is set using a tool set switch with is within the .005" range too. To get around the y problem I have written a small program that cuts a slot 1" long from either side of a piece held in the a axis and rotated 180 for cuts to be made from either side. I then measure the difference of the cuts, divide by 2 and move the y axis to the correct dro reading.

Now for sake of time let's assume my known correct position is:
x27.200y108.4724z-2.125a0.000 BTW this is my know position today.

The tool length set switch uses a G92 to set the tool tip at a know distance from the centerline of the a axis. This macro also sets the z axis dro to 0.000 G92 is modal so it is in effect till it is canceled, but presently only in the z axis.

All my programs are written from x0.00y0.00 with whatever z I need, and there is a G92X0.00Y0.00Z0.00A0.00 used about 5 lines into my programs to set all dro's to zero.

With this info, can anyone take the time to explain in very plain English how to do this with the offsets other than G92. It is possible to have a new tool set macro that does not use G92, so please take that into consideration.

I know this is more like a book, but I only want to have to learn this stuff one more time! Thanks in advance to anyone willing to help.

Mike
__________________
No greater love can a man have than this, that he give his life for a friend. "

Any help would sure be appreciated.

Mike
Re: G54 offsets questions
« Reply #1 on: August 12, 2006, 10:42:09 PM »
No one? :'(

Offline Graham Waterworth

*
  • *
  •  2,394 2,394
  • Yorkshire Dales, England
    • View Profile
Re: G54 offsets questions
« Reply #2 on: August 13, 2006, 04:48:35 AM »
Hi Mike,

there is nothing wrong with using G92 as a datum point, that is what it is for,  changing to G54 will not improve the accuracy of the homing switches.  The main advantage of using G54-G59 is that you can change from one datum point to another in program.

e.g.

If you have two fixtures on your table you can have one datum at G54 and the second one on datum G55.  The code would be something like this :-

G20 G40 G80 Etc
(STANDARD SETUP LINES)
G54 G00 G90 G43 X0 Y0 Z1. H1 (MOVE TO FIXTURE 1 AND DRILL A HOLE AT X0 Y0)
S1000 M3
Z.1
G01 Z-.25 F2.
G00 Z1.
G55 X0 Y1. Z1. (MOVE TO SECOND FIXTURE AND DRILL A HOLE AT X0 Y1.)
Z.1
G01 Z-.25 F2.
G00 Z1.
M30

To set the fixture datums you go to 'Operator' and 'Fixtures' off the window menu.  You will see listed in the new window a list down the left hand side the top 6 are marked G54 to G59 all you have to do is set your X,Y,Z,A values into the corresponding row.  These values are the same as the known position for your G92

Remove all G92 commands from your code including the X,Y,Z and A and just enter a G54 instead.  This will then tell mach to use the G54 datums stored in the fixture list.

The advantage of this is that if you have more than one program that uses your indexer and the datum point for each program is the same then you don't have to worry about changing the G92's in each program.  They will all use the same G54 setting in the fixture list.

I hope this helps.

Graham.


Without engineers the world stops
Re: G54 offsets questions
« Reply #3 on: August 13, 2006, 10:27:39 AM »
Thanks Graham,

Now I understand a little better. I have just changed to mach3, or actually in the process, and wanted to go ahead and change all my system to better work with mach3........but for now I'm, going to keep the G92. I don't like it due to it being active till cancelled. I have on occasion had to quit a program in the middle somewhere and forget that the end of the program had not canceled the G92  command only to ruin a part or bit.  Thanks again for your help.

Mike

Offline Graham Waterworth

*
  • *
  •  2,394 2,394
  • Yorkshire Dales, England
    • View Profile
Re: G54 offsets questions
« Reply #4 on: August 14, 2006, 04:46:15 AM »
Mike,

G54 is also active just the same way as G92.

Graham.
Without engineers the world stops
Re: G54 offsets questions
« Reply #5 on: August 14, 2006, 03:32:28 PM »
Hi Graham,

I understand that about G54, but unless I am mistaken, an active G92 will take precedent over the G54. Meaning of course, that whatever the G92 set the dro's to will remain persistant until cancelled. I did get a reply from over on the Zone from a fella that I have a lot of confidence in and he basically told me that till I got my unstable homing issue corrected  in the y axis that the G92 was still probably gonna be my best bet.

Mike