[yukonho]

I am a bit confused. Usually I zero my axes to indicate where my part is on the machine, I run in absolute mode.
With machines with homing switches, the machine is homed to the limits of the axes. How do you then tell the machine where the part home is, and still have it know where the machine home is?
I am guessing that you would then run in incremental mode, but I really dont know. Can anyone shed some light?
Thanks.
Colin

[Karl_T]

I'm not a Mach user, but virtually all controls handle this situation by have both a machine coordinate system and a part coordinate sytem. Some have more than one part coordinate. This allows you to still use absolute, G90

Look in your manual under G54 and G92.

Karl

[ger21]

Mach3 by default is usually in G54 coordinate system. Go to the offsets screen and you can set up offsets which will set up your part zero wherever you want. Just call the correct cooedinate system before you run the part, either with MDI mode, or put it in the g-code. After switching offsets, clicking the "machine coordinates" button will show you where you are inrelation to your home switches.


On our commercial router at work, there are stops to locate the workpiece at 0,0 every time. You can do the same thing with Mach3 by setting your G55-G59 offsets so that 0,0 is where you put your part, and useing some type of referencing fixture to locate the part on the machine. Don't use G54, because the G54 offsets are changed whenever you use the zero axis buttons. If most of your parts can be run from the same 0,0 location, set that up as G55. Then, if you need to run a part somewhere else on the machine, use G54 and jog to position and use the zero buttons.

Hope this makes sense.

[yukonho]

Thanks guys. It all makes sense.
Cheers,
Colin

[HuFlungDung]

I think industry standard is that G53 is the machine's coordinate system. G54 is the first work offset. I don't know if Mach follows this convention or not?

When you home the machine, that sets the machine zero of the G53 coordinate system. This is actually the only 'real' coordinate system that there is, all the work offsets are relative to the G53. Whatever values you see in your work offset tables are actually coordinates in the G53 coordinate system. The G54 through G59 coordinates are the location of a temporary shift in position of the current part's coordinate system origin from machine 0,0,0 to that newly named position.

[ger21]

I think industry standard is that G53 is the machine's coordinate system. G54 is the first work offset. I don't know if Mach follows this convention or not?

Yes, it does.