CNC Router V1.0 (For Cutting Multiple Materials)

[JAZZCNC]

M_C answered most of it but here's couple more suggestions.

1. A: Good Habbit to get into starts at the Cad when you define the part. I always place it 2 or 3mm in from X0Y0 then when you touch off the billet side you know you'll always be inside it and won't run off the edge.
B:Another way is to draw the outline of the billet in cad and have X0Y0 on the corner and work piece inside it.

2. Easy way for one-off's if working from square/rectangular billet is to use the billet corner has X0Y0 like in option B: above then when you flip just make sure the edge is parallel to Axis and pick up X0Y0 from corner again.
Problem comes when you can't work from square/rec stock or if need to relocate already completely machined parts.?
In this case then it's often better to place X0 Y0 in cad on a hole centre or other defining feature that's easily picked up off using touch probe or other manual technique.

Regards the touch probe then doesn't need to be any fancy or expensive tool just piece of wire with plate on the end of a known thickness and using a spare input setup in the control has probe input. Then put plate between tool and work piece.
So long has the tool diameter is known you can just use what ever tool is in the spindle for quick touch off, if you want very accurate position then best to use accurately known shaft or tool shank.
(Tip: If your working with Ali or metals and can isolate the work piece from the main frame or Ground then you don't even need to put the plate between the tool and work piece so can enter just tool radius into DRO for offset. Just touch probe wire to work piece.)

This can then be used in few ways either by using the G31 probe command directly and telling it the axis direction and distance to travel looking for the edge.
Then when it's touched off you zero the Axis DRO's and type the radius of the cutter + plate thickness directly into the Axis DRO to give correct offset from edge.

To find hole centres you'd do this for each X,Y axis if you know the hole radius then type that minus the cutter radius + plate thickness has either positive or negative value depending on which side of hole you probed has the new offset.

With that said the best way and easiest way when it comes to probing is to use pre designed scripts with probe commands etc for each type of probe routine you want to do which does all the offsets etc for you then add a button to your screen set so it's a one click affair.! . . . OR . . .
By far the best and easier way if you use Mach3 is just buy Gerry's 2010 screen set which has all the probe routines you'll need and more besides. The CNC Woodworker - Mach3 2010
With this screen set and simple touch plate on wire you'll very accurately find most locations and will be the best £15 you ever spent.