Post processor with THC and floating head.

Problems and questions
1

Hello.

I am very new to sheetcam and I am trying to setup my program. I am trying to chose a post processor. My CNC setup is currently from Planet CNC and I am using a MK3 board.

I have been looking at the Mach 3 plasma TCH with scriber and backlash compensation.

But it seems that this is featuring “Floating head Touch-n-Go” as far as I understand this is based on an ohmic sensor?

My setup has a microswitch witch is activated when the torch touches the material and lifts the torch.

Am I able to use this processor or should I chose something else? I don’t need the scriber either but I thought this processor was the one most suited to my use.

Anyone have any suggestions?

Thanks,

Mr. Emo

2

The “floating head” is for your micro-switch. That post will probably work for your machine. You will have to do some setup work in the post, such as your micro-switch offset.

If the post doesn’t work, then you can always try something else.

Steve

3

I’ve been testing a little bit now and it seems to work ok.

But I have some concerns about the floating head. It doesn’t seem to work?
I set my offset to 2.5mm

There is a post:
–If this value is set to true then use G28 (home) for the Z reference
–Set it to false for G31 probe
refHome = true

Is this what enables/disables the function of the micro-switch? Should this be false so the machine uses G31 instead?

Should I then setup my sensor as a “probe” in the planet cnc software would that be sufficient?

I know this probably should be addressed on the planet cnc forum but they are really slow at answering.

4

Apparently Planet CNC software doesn’t recognize the code G31. So that definitly doesn’t work.

Any suggestions to other post processors that would work with this software or do I have to rewrite the processor?

5

The Z should go down until it touches the material, then continue for a little bit (the switch offset) until the switch operates, at which time the Z will go back up until the switch opens. Then the Z DRO should zero out. When the switch operates, you should be able to see the bit light up on the diagnostics page.

You should be able to raise the torch mount by hand and see the bit operate on the diagnostics page. If it doesn’t light up, then you need to check your wiring and options.

Steve

6

I have also use the PlanetCNC Mk3 and in sheetcam i use the LinuxCNC THC.
And you have to switch the seek code from G38.2 Z-1.75 F10 to G10 L7 R17.5. The R in the command is the offset for my floating head. And you have to delete these 2 lines

Code:
function Reference()
firstRef = false
post.Text(seekCode … “\n”)
post.ModalText(" G92 Z")
post.Number(-switchOffset * scale, “0.0###”)
post.Eol()
post.CancelModalNumbers()
end

and change it to
Code:
function Reference()
firstRef = false
post.Text(seekCode … “\n”)
post.Eol()
post.CancelModalNumbers()
end

7

Thank you! That seemed to work ok. :slight_smile: