G54 offsets questions

[turmite]

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

[HuFlungDung]

In the situation you have described, I don't think there is anything wrong with using a G92, indeed, it is almost necessary to do so, because of the 'float' in your machine whenever it homes on starting up.

It might be an idea to create a fixed reference point on your machine that you could dial in with a dial indicator. Suppose you were to permanently drill an accurately round hole in the table somewhere, but on purpose

After starting up your machine, you could check this location by centering the spindle over the hole with a swing indicator.

Even then, once you have done that, you will have to use a G92 X0Y0 command in MDI to set the machine position at that location. Essentially what you have done is renamed the coordinates in the machine coordinate system, which is G53.

Now, the location of your part, A axis or whatever, will be certain, and repeatable from that point onwards. Assigning a work offset simply becomes a matter of measuring the exact XY displacement of your desired work zero, back to the machine reference "hole".

You might also need a fixed height bar to set the machine's Z axis to zero. For instance, this could be almost the maximum distance from your spindle nose to the tabletop. Tool length offsets take care of the individual tools, of course.

Your Z axis work offset might be set differently. If you set all your tool length offsets off the table top (or a guage block sitting on the table, same diff), then the Z axis work offset would be the distance from the table top to the part's Z zero surface. In the case of 4th axis work, this would typically be the centerline height of your A axis. I am assuming that you call the centerline height Z zero in your part program, but that is your option and could be set somewhere else.