UGS Return to Zero

lol, on some advanced machines, like Haas, there are advanced Gcodes for this sort of thing.
for GRBL, you just have to send it the correct Gcodes, so somehow we need to convince UGS to do it
OR
we need to put the right stuff in our post-processor the makes our Gcode.

Let me deal with what I know well, SketchUcam.
Normal operation for Sketchucam is tohave the top of the material as Z-zero
you also set a 'safe height' value in the parameters, and all Z motion that is not cutting will happen at that safe height.
So if you have vacuum hold down and no clamps, this can be 1mm above the material (if you dare), 5 or 10mm is more common.
If you are using clamps, then this safe height should be set to clear the highest point on the clamps, ensuring that Z will always retract far enough to miss the clamps during rapids.

great so far, but what about the end of the job?
The default is to return to X0 Y0 Zsafeheight, like this

Code:

G90 G21 G49  G17
M3 S30000
G00 Z5.000         ; safe height
G00 X55.657 Y50.763
G00 Z0.500         ; rapid to near the surface
G01 Z-6.300 F1000   ; cut down into the material
G01 X174.057 F2000
G01 Y139.463
G01 X55.657
G01 Y50.763
G00 Z5.000       ; rapid up to safe height
G00 X0 Y0 (home)   ; return to zero, safely

Let us now consider some options we can use for the ed of the job.
If you are using a Phlatprinter, the default will make the foam stick out the BACK of the machine
If you set Use_Outfeed to true in the Feature Options, the foam will feed 3/4 of the safe X size out the front of the machine at the end of the job.

Code:

G00 Z5.000
(Outfeed)
G00 X150.000 Y0.000

That is not useful on an OX type machine....
So, let us put values in for

• Use_Home_Height/Default_Home_Height
• Use_End_Position/End PositionX/End Position Y

Now the ending for the file will put Z at the given home height, and X,Y at the given values. I would use this for moving the gantry
back, away from the material, so I can get my parts out easily.
There is one snag with this in that such movement will be limited by the current safe area.
Here I have set the end position to 300,300 and 32mm high, but my safe area is 200,200, so we get working code with warnings in it.

Code:

cut cut cut....
G00 Z5.000
(EndPosition)
(Warning move x=300.0mm GT max of 200.0mm)
(Warning move Y=300.0mm GT max of 200.0mm)
G00 X200.000 Y200.000 Z32.000

This is ok though, the bit will move to 32mm above the stock at the far right corner, out of our way, just as we wanted.
To move it further away, either change the safearea, or be prepared to do some manual editing to something like this

Code:

G00 Z5.000
(edited EndPosition)
G53 G00 X400.000 Y500.000 Z0.000

now the machine moves in machine co-ordinates (G53), ignoring your current X0Y0 setting, so you have to be sure you have
the correct numbers in there. GRBL likes to find home switches at far right of the cutting area, so that is machine 0,0,0 so be very careful with these numbers.

so, back to UGS, let me fire it up and see..... (they call me a geek cos I have an Arduino with GRBL in my office so I can work with it directly without having to forget about it until I get home)
on the Machine Control tab, when you hit the 'return to zero' button it sends the machine to the machine co-ordinates set for G28, normally 0,0, actually outputting the Gcode

Code:

G21 G90 G0 Z0.0
G90 G28 X0 Y0

effectively sending Z to 0
and X and Y to machine 0,0 AFTER Z has moved.
This is not what we want, as you pointed out.

so, UGS is open source, and you can grab all the code and go and find the button action for 'return to zero' and change the code, recompile, reinstall etc etc. can be done, Java is not that hard to deal with.
OR
you can use the 'macros' tab and set up a macro to do what you want.....

Code:

G90; G53 Z0; G53 X0 Y0

will send it to machine 0,0,0, moving Z up first (machine Z zero should be top of Z travel)
or we can use the g28 position and machine zero

Code:

G90; G53 Z0; G28 X0 Y0

or some position that suites your setup, you will need to figure out the correct numbers, example:

Code:

G90; G0 Z100; G0 X200 Y400

glossary:

• G90 - changes movement mode to absolute, just in case your last program used relative
• G53 forces use of machine position, otherwise all movements will use 'work position', only lasts for the current line
• Machine position or 'machine co-ordinates' : where the machine thinks home is
• Work position : where you used 'reset X axis' 'reset Y axis' etc to tell the machine where 0,0,0 on the stock is. By default this sets the G54 system unless you change it to G55 to G59