G54 vs G43 offsets

I'm retrofitting an EMCO 120 and my home position is at the upper right corner of the machine. This puts my main turning tool about 85mm to the right of a part in the chuck and about 42mm above the centerline of the spindle. I think I understand the interaction of the G54 coord space and the G43 tool offset but I wonder which one contains the bulk of the 85mm between home and the end of the part. Should the z offset in the tool table for this tool be 0 and the z offsets for other tools be referenced to this? That would mean that X offset variable for G54 would be something like -85mm.

I've read the writeup here: gnipsel.com/linuxcnc/g-code/index.html The sequence seems to be setup G54, set G43 tool offsets and then do the material offset but I don't understand what makes good G54 offsets for XZ on a lathe. The writeup mentions picking up offsets on the fixture for a mill but what works well for a lathe? And what tool should I use.

Sorry if this is straight forward to other people but I'm having a tough time wrapping my head around it.

Drew

Hi

The distance from the home position to the chuck is of no relevance regards tool offsets.

Home is a G53 position 0,0 from which G54 etc are offset, but this is not related to the tool offsets, which are relative to each other.

Simplest method I use.

Home, choose tool 1 and touch off on a known sized billet to Xknown diameter, Z0 in G54
I actually have an insulated 12mm rod with a walmart PSU, and a LED which lights on contact with the tool tip on the rod.

Then move away and select tool 2
Come back down and touch off (but don't zero the DROs). The difference between the figures is the offsets from Tool 1.

And so forth

All the offsets are the same no matter what co-ordinate mode you are in, because they relate to the tools variation from tool 1, not the position of the axes.

When starting a job, home then come down to the billet and touch off with Tool 1 so that the tip is just touches on the billet
Take a very light cut in the X plane to establish Z0 and touch off (zero the DRO)
Then take a light cut in the Z plane and measure the billet after the cut accurately and touch off X to that figure.

Now return to home and select whatever tool you require, apply G43 and if you have set up accurately, commanding G0 Xdiameter Z0 will take you to exactly the same place with the new tool.

Hope that is clearer?

regards

ArcEye wrote:

Hi

The distance from the home position to the chuck is of no relevance regards tool offsets.

Home is a G53 position 0,0 from which G54 etc are offset, but this is not related to the tool offsets, which are relative to each other.

Simplest method I use.

Home, choose tool 1 and touch off on a known sized billet to Xknown diameter, Z0 in G54
I actually have an insulated 12mm rod with a walmart PSU, and a LED which lights on contact with the tool tip on the rod.

Thanks ArcEye. So you just leave the XZ G54 offsets at 0, 0? I tried that today and it worked after I set my MIN/MAX_LIMITS in my .ini file to +-80 in X and +-115 in Z. For sake of discussion, the magnitude of the numbers don't matter but I was surprised that I had to have both plus and minus given that my home location is at the maximum X and Z. I'm going to verify that I actually need the -values tomorrow..

Then move away and select tool 2
Come back down and touch off (but don't zero the DROs). The difference between the figures is the offsets from Tool 1.

And so forth

All the offsets are the same no matter what co-ordinate mode you are in, because they relate to the tools variation from tool 1, not the position of the axes.

When starting a job, home then come down to the billet and touch off with Tool 1 so that the tip is just touches on the billet
Take a very light cut in the X plane to establish Z0 and touch off (zero the DRO)
Then take a light cut in the Z plane and measure the billet after the cut accurately and touch off X to that figure.

Now return to home and select whatever tool you require, apply G43 and if you have set up accurately, commanding G0 Xdiameter Z0 will take you to exactly the same place with the new tool.

Hope that is clearer?

regards

It helps but why do I need to re-touchoff the X to the material. I would assume that the tool X offsets wouldn't ever change.

Drew

For sake of discussion, the magnitude of the numbers don't matter but I was surprised that I had to have both plus and minus given that my home location is at the maximum X and Z. I'm going to verify that I actually need the -values tomorrow..

I have a slant bed lathe, my MAX_LIMIT on both axes is set to +0.5 ie half a mm beyond the home position but short of the limit switch.
The MIN_LIMIT is set to -150 on the X axis and I have various setting for the Z axis, depending upon which chuck I have mounted (between -140 and -93 when using forward tooling)

The limits operate in machine co-ordinates so it is the distance from home at 0,0.

..............why do I need to re-touchoff the X to the material. I would assume that the tool X offsets wouldn't ever change.

There are some that say exactly that.

The tool offsets don't change, but they are in relation to tool 1 not the workpiece, the crux is whether the absolute position of tool 1 in relation to the Z plane changes

If your X home position is consistant to within the workpiece tolerances that you work in and your tool never wears or wear is compensated for, that argument holds.

I only turn one-offs. I want them to be exact size.

The answer is to test. Mount a billet and take a light cut and then measure it. Set the measurement in the DROs

Then switch off, switch back on, re-home and go back to the billet and take another cut and measure again

Does the measurement match the DROs?

regards