Questions on using a moving gantry style mini-mill...

[Davek0974]

Thanks for that, explains a lot then ;) Don't think I've ever used RFH...reaches for manual ;)

I think for what I am doing - small batch production - saving the offsets is a good idea??

All the raw plates are pre-cut to the same size and pre-drilled for fixing to the bed so each part will always start in the same position or work-offset.

Is that what offsets are for?

Could I then have re-homed the machine and loaded the offset then carried on with part I had stopped on??

Lots to learn....

[Ger21]

If you don't close Mach3, the offsets should still remain after homing. (I think)
Yes, if you have a specific part that you always run in the same place, use an offset like G55,G56,G57...
Add the G -code to the beginning of your code, and save the offsets. Then when you turn on your machine, you just home, load the code and run.

[Davek0974]

Sounds good, an offset will do what i need, i have never checked if the work position remains after a home, something else to check.

[JAZZCNC]

Sounds good, an offset will do what i need, i have never checked if the work position remains after a home, something else to check.

Yes it does offsets are Modal so will only change if you set a different offset. G54 being default so if you don't save the Fixture offset when closing Mach3 it will always load the previous G54 offset which was saved.

Regards Homing and Stop. It actually goes further than that regards homing. If you have stopped the G-code with feedhold and in controlled manner then if you for any reason power down the drives, which a safe E-stop system should. Then you should home the machine when they power back up.?
This is because they often jump to next full Step so your then out of positon to where mach thinks it is.

Then if your trying to get back to position use RFH. I use RFH all the time it's a great tools when shit hits the Fan.!!!

[Davek0974]

Great stuff,

If I'm using say G55 for my job, it will still be there next time i load?? That sounds like a recipe for fun ;) Can it be programmed to always load into G54?

The G55 could/should be added to the start of the specific G-Code file?

Stuff to learn...

[JAZZCNC]

If you save the Offsets when closing or by Saving directly in work offsets then G55 will be saved but by default Mach on start up will load G54 so your safe.
If you want G55 or any other offset you'll have to call it with MDI or Thru G-code.

To use different Offset with in one G-code file you'll first need to create the offset and save it.

To see it work Try this.!!
By default your in G54 so set Zero work coordinate. Then Type G55 in MDI now jog away and set Zero again in different place.

Now in MDi Type G54 G0 x0 y0 and it will got back to zero you set for G54. Now type G55 G0 x0 y0 and it will go back to zero for G55.

So say you have one part you need to make but in two different materials. First set up the Zero Offsets for each material G54 & G55.
Then use copy and paste. The first part will most likely have G54 at the begining by default. So paste the code again for the second part and replace G54 with G55.

Now when code runs and gets to second run of part it will use the new Zero at G55.

If you want to keep thses offsets then go into Offests and save work offsets.
To be honest saving Offsets before starting job is a good habbit to get into because if Mach crashes or PC then you lose the offsets and have no way easy way to get back into position. This happens often with parallel port machines when being run hard.

[Davek0974]

Excellent, that makes sense.

I have "optional offset save" turned off so it only saves what i want to save into the offset table.

I don't think sheetcam has a work offset option so it'll have to be a manual add, but can't have everything i guess ;)