[The Engine Guy]

New flexible couplers have been installed, along with complete cable replacement due to splices in middle of old ones and
sheath grounded on both ends(motors and controller box). New ones sheaths are only grounded on controller box end to
hopefully eliminate any EMI from power and control cables running side by side in cable trough. With changing the G54
to G56 and adding a G0Z5 below that mill is performing very well on fusion 360 gcode. I still feel more comfortable working
with a G56 offset somewhere near middle of table for now. Motor pin connectors were exposed and prone to be struck by
accident without extreme care, so I have designed some guards and will post pics soon of what that looks like. In near
future I am the removing the mdf mill bed and replacing with 1.5 inch delrin plate topped with 1/2 inch aluminum
plate drilled every two inches with 1/4 threaded holes for holddowns. At that point I hope to try some aluminum milling, which
will include either air pressure mister or cutting fluid mister. Thanks for the help in getting me pointed in the correct
direction.
Anthony

Don`t know what type of Motion Controller you are using but if it is one of the type that runs off 5 Volts USB then it will be very prone to interference, always best to use an industrial type that runs off 24 Volts, way better.
I see you have sheathed your cables which is good but the best way to cut down/eliminate interference is to use the "twisted pair" system for cabling, especially for signal wiring going from your Motion Controller to the Motor Drives, a good example is an Ethernet cable, if you have any old ones lying about they are excellent for getting your "step-direction" signals to your drives.

The G56 has nothing to do with the machines Home position, it is, as has already been shown (mactec54) simply a distance that is a reference from your machine Home position, so here is an example, jog your machine in the X and Y to say the lower left corner of you machines travels and your Z axis to it`s highest point and now set your Machine Zero at that point in Mach3, to make sure it is working correctly now jog your machine away from that position in all three axis, doesn`t have to be far, and then click the "Ref All Home" button, your machine should now run back to the original position, do it a few times to be sure, the machine should return to that position every time, your machine is now "Homed" and should not need changing again so set all your DROs to Zero. Now set your soft limits to the values you originally jogged to. If you have proper Limit Switches on you machine then you can of course Home to them, if not go as above.
Now, to get your G56 for example place your vise/piece of stock (if using clamps) on the bed and using the "Offsets" tab in Mach3 first select the "Active Work Offset" you wish to use in this case G56, now using all the probing system on that screen set your G56 to say the Lower Left corner and top surface of the stock. Go to your "Fixtures" area in Mach3 and check that the X,Y and Z values for your probing are showing in your G56 offset in the table.
When that is done on the same screen do your tool offsets so all your tool lengths are stored in your tool library and go double check them also.
You should be good to go now, the tool offsets and the G56 Work Offset are stored so even if you turn Mach3 off they are remembered, so if you want to do a different job at at different position on your table you would only need to do the X,Y and Z probe for say G57.
Using the Homing system gives you proper repeatability and much easier setting up from then on as every time you turn the machine on you only need to press the "Ref All Home" button and the machine will run to it`s Home position ready to start work straight away
One small tip, if you are looking to machine metals then make sure that your tool are really tight in the spindle as they can be easily pulled out of collet chucks !!

Hope that is of some help to you
Regards
Rob