Creating a button to trigger an output on the mach 3 screen

Hey guys, I built my machine the way ToolJunkie on youtube did his. I just wired in the thc override and was wondering how you guys create the button with the macro to trigger the output or better yet, if someone had the tooljunkie screen file. I downloaded screen4 but cant figure out exactly what does what

What is this ‘thc override’ supposed to do? I don’t have it on my machine and, apparently, don’t miss it…

I have a z axis and an external THC. The THC override is connected to a relay that disconnects the arc voltage reference for the torch height controller and disables the THC

Ok, but why do you need this? For debugging?

FWIW, I also have Z Axis and THC (THC3T-02) on my CrossFire and do not have this override. I don’t need it. If I want to make a cut without THC active (like when I’m doing a new material and I don’t know the proper settings), I simply set the THC threshold higher than it could possibly get during the test. The advantage of this is that I can watch the run and see what the nominal value is during the cut - I can’t do that if THC is disconnected from the Torch.
Now, your question is an interesting one for other possible purposes (like Water Fill/Drain control to take a random example), but I don’t see a need for THC.

I cut alot of parts with small holes, etc where being able to disable the thc for those would be a huge help since your cut speeds are lower. I have the same thc as you and always have issues with the torch diving at the end of the part as well which drives me nuts. I cant figure out what sensitivity settings are low and high on it

I’ll dig up my settings tomorrow and post them…

Ok, fair enough, but wouldn’t you rather have your G-Code control the THC on or off in that case?
If yes, then I’ll post something to help you out tomorrow.
Do you use SheetCam or Fusion360?

Yes that would be awesome. I guess that’s what I’ve been trying to accomplish but also have a way of doing it manually as well. I’ve been using fusion but will probably upgrade to sheetcam evenually

My understanding of the THC3T parameters is:

  • U is the ‘target’ voltage. This is what the THC will attempt to maintain while cutting by adjusting Z Up and Down to keep the Z height exactly at your target. This is controlled by your Pot for each kind of material you’re cutting.
  • A is not hysteresis, but a ‘window’. The THC will try to compensate ONLY if the voltage is inside the window, otherwise it doesn’t adjust Z. The Window is U-A to U+A. My A value is 20.
  • S is sensitivity of the correction. 50 works well for me after I tuned V and A. It controls how many steps it generates to correct the voltage error.
  • V is the maximum stepping speed the THC will send to your Z Stepper. It’s sort of vague unit-less value, but I reduced it by a factor of 3, from the default ‘30’ value, because the step resolution of my Z Axis is one third of my X & Y settings and, consequently, moves faster than the X & Y axis per step. That relationship works well for me.
  • D is delay in 10th seconds from when the THC ‘sees’ an ARC to when it starts compensating. D is short in my case (D=8) because my window (A) is relatively narrow and this value covers most pierce delays and getting the gantry moving. I make sure the voltage is within the window and then respond quickly. Tuning the other parameters keeps the torch operating within just a few volts. Very nice cutting.

Note that, in your case, you may be able to set the D value longer to avoid responding when cutting small holes. If you’re calibrating Z (AKA IHS) at every hole, then chances are you don’t need THC to kick in right away and you can set it to something like: D = 8 + ROUND((Dia*Pi)/IPM)*600), where Dia is the largest hole size you want to skip THC (in inches), Pi is Pi, IPM is your cutting speed, and 600 converts the time from minutes to 10th seconds.

FWIW, I don’t use the Plasma Cutter to cut small holes. I ‘drill’ them with just a ‘peck’ in the center of the hole and actually drill them after cutting. I don’t like the holes the PC cuts and definitely don’t like the hardening you get with plasma cut steel.

1 Like

That’s too bad :wink:
because I could give you two ways to deal with this with SheetCam, but I’m not really able to offer a suggestion to have Fusion add this to your G-Code automatically. In this case you’d have to manually modify the G-Code to add the THC OFF & ON commands. This isn’t SO bad if you group ALL of your small holes in the first operations because you’d only have to add OFF to the beginning of the block and ON at the end.

In any case, like practically anything in Mach 3 there are bunches of ways to do things. The ABSOLUTE simplest way is to use M7 or M8 to set THC OFF (assuming you want ON as the default) and M9 to set THC ON. Mach 3 Configuration will Map M7 and M8 to an OUTn signal of your choice and will turn off this OUTn signal on start up and when M9 is executed.

This configuration is in:
Config->Ports & Pins->Spindle Setup
Under Flood Mist control, you will find settings for M7 and M8. If you uncheck ‘Disable Flood/Mist Relays’ and then modify either Mist or Flood setting to 2,3, or 4, then using the M7 command, for example, with turn ON the corresponding OUT signal (Note, OUT1 is already used in CF as Torch On).
Then in the Output Signals tab, you need to enable Output #n and set the Port & Pin number. Note that, in keeping with Mach 3’s attempt to confuse everybody, the Pin numbers are reversed from what you’d expect and OUT1 is pin 4, OUT2 is pin 3, etc. The port is always 3. You can invert the sense of the output so that the output is HIGH when ON by checking ‘Active Low’ (another feechur of the Mach 3 hardware).
I’ll stop here, as this should be enough to confuse you, but, if not, ask more…

1 Like