Plasma Z floating head

[happytriger2000]

Hello,
        This is my 1st post in Machsupport.
I have a 3 axis cnc router and  I want to convert it to a plasma machine, so far this is what I have done:

http://s1220.photobucket.com/albums/dd459/happytriger2000/Machsupport/?action=view&current=M4H02695.mp4
I wan the Z axis to do the same as in this video:

http://asooke.com/videos-cnc-plasma-with-thc-and-floating-%5Ban5HYBQWTpg%5D.cfm

Can anyone guide me from this point onwards?

thanks,

[BR549]

You can set it up one of two ways using the G28.1 method OR use the G31 method.

With the G28.1 method you set up your floating head as the Z home and have it  home toward the bed. Then the Cam that you use must generate the following type code.

N0120 G28.1 Z0.50
N0130 G92 Z0.0
N0140 G00 Z0.1370
N0150 G92 Z0.0
N0160 G00 Z0.2000

With the G31 method you setup the floating head as a Probe then you cam must generate code like

N0120 G31 Z -100 F19.685
N0130 G92 Z-0.0800
N0140 G00 X5.5505 Y9.8813
N0150 Z0.0000


Hope that helps, (;-) TP

[happytriger2000]

Hi Br549,
             Thanks.


I'm still hesitating on what the exact vulue should it be for the distance between the MicroSwitch and the Torch collar?
Currently is 13.7mm.

Should this distance be the thickness of the plate that going to be cut, 6mm,?

thanks,

[BR549]

That distance PLUS the amount of travel in the switch is used to move the head BACK up so the tip of the torch is exactly at the top of the material.

Using the G28.1 method and assuming the distance + the travel equals .250"  NOTE: your Cam program will have a place for THAT setting

G28.1 Z.50   ' references the head down until it trips the switch
G92 Z0.000   'Sets that point to ZERO
G0 Z0.250     ' Moves the head UP the amount of the head travel + switch movement
G92 Z0.000   ' Sets that position to ZERO, that will be TOP of the material,
G0 Z.100       ' Move the head up to a clearance position

NOW you head is referenced to the TOM and you are ready to start a cut.  

Note that most CAMS rereference the TOM every so many inches of torch travel . If the setting is every 50" then the next torch start after the machine has cut 50" then it will ref the head before it cuts again.

Collar Distance?? Make it anything you like (;-) normally  the closer the better.

Hope that helps (;-) TP  

[happytriger2000]

Thanks again BR549,
                             
I'm new to Sheetcam, still using a demo version downloaded yesterday.
I was wondering if it's possible to use Mach 3 to do the Z axsi floating offset without Sheetcam?.
Like the Mach blue screenset that has the Autotool zero feature, Link:http://www.cnczone.com/forums/cnc_wood_router_project_log/36099-another_aussie_auto_tool_zero.html,
instead of touching the plate,  Z home switch is tripped, reset Z DRO to zero, raise Z to Swtichoffset value so tip is setting on top of material, reset Z to zero as top of material, raise Z to pierce height, fire torch.

I haven't used a plasma machine before, only hand cut.

[BR549]

It would be best to let the Gcode side drive that part and use Sheet Cam to post the code. At that point it is an automatic function.

(;-) TP

[rrc1962]

I use a macro in Mach3 to handle the torch referencing.  I use one of 3 methods for sensing.  Ohmic, floating head or capacitance.  The machine is set up with all 3 and I never really know which one I'll use, so in Sheetcam I just insert the M code for the macro.  Each method uses a different offset. The macro looks at a few different parameters to determine which method is in use and runs the referencing routine.  After the macro runs, M03 is called to fire the torch.

If pierceHeight <= 0 Then
   MsgBox("Please enter a valid pierce height")
   code "M30"
Else
   code "F30"
   code "G31 Z-1"
   While ismoving
   Wend
   code "G92 Z" & offset
   While ismoving
   Wend
   code "G00 Z" & pierceHeight
   While ismoving
   Wend
End If   

[happytriger2000]

rrc1962,
           Will try your code, I kind of forgot how to edit the M03 code, please guide me,

Thanks,

[happytriger2000]

Ok I think I know,

C:\Mach3\macros\Mach3Mill

[happytriger2000]

rrc1962,
            I entered the code in M03, when I test run .nc file, when M03 is called I was asked to enter a  valid pierce geight, and where do I put this pierce height value?