A little background: first few cuts with the machine I got the “arc voltage lost” error, and was able to fix those errors with a combination of the THC firmware updates, as well as the ferrite choke on the USB cable. Since then, I’ve been able to run programs without freezing FireControl or having any error messages.
Now, the problem: I was cutting some 1/2" plate yesterday and not once did the torch adjust the height while cutting. THC module is definitely connected, has the latest firmware (v1.05), and does not have the continuity issue addressed recently about the USB housing and control board nuts. Voltage is displaying correctly in the “live” area, SmartVoltage is being set correctly, and my tolerance is set to plus/minus 1.5v. As I watch that section of FireContral during cutting, none of the 4 “lights” in the THC window (active, ok, up, down) ever illuminate. Even when the voltage displayed is outside the tolerance window. (last night I saw 118v when smart voltage was auto set to 112v) or when it is within that tolerance. I then started watching the motor coupler on the Z-axis during cutting to see if it was adjusting, but just not showing in FireControl. Turns out, it wasn’t moving at all either.
Any ideas?
Thanks!
Hi @golferguy17 can you attach your program here? I suspect that your program speed PS value at the bottom of your program might be the culprit. THC only comes on active when the current live cutting speed exceeds the programed speed multiplied by the Torch Speed Cutoff Factor (in the settings). On that note, what is your Torch Speed Cutoff Factor set to?
@langmuir-mike In sheetcam I have the perimeter cut set to 30ipm, and the slotted holes at 18ipm. The cutoff factor is still at default, which is 85%. All THC Settings are default as well.
4 Slot Notched Corner Plate 1st 8 parts.tap (17.7 KB)
Hi @golferguy17 I see the issue in your g-code. Go to the last line and manually change this value in a text editor to (PS18) and you will see the THC come on. We still have some edge cases to fix in our SheetCAM post and this is one of them (using two different cutting speeds in the same program)
@langmuir-mike Well damn! I did notice the PS100 code at the end of my files but had no idea what it meant. (I was editing the code to manually add a 1 minute pause after each part to let my compressor catch up… a feature I’d like to suggest for the future. Sheetcam allows you to pause after each cut, but that keeps your torch blowing into the water below and splashing. It’s much better to move to the pierce point on the next cut/part, and then pause over fresh plate… Ok tangent over)
I’ll go edit that now. All of my programs so far have had 2 cutting speeds (holes/perimeter), so I doubt I’ve ever actually used the THC! Surprised I’ve gotten the results I have even with it off haha.
So do I need to manually do this for each program until an updated post is released for sheetcam?
That cut looks fantastic! Fortunately since the IHS sets the correct height at each cut loop and that part is small, THC probably wouldn’t be doing too much anyway. You can really see it working a lot on thinner material and longer cuts.
For now I would edit this value by hand; we are working on the post fix this week so hopefully we will have something for you soon!
@langmuir-mike Is a 12" x 13" x 1/2" plate considered small? 
So should I set it to the lower of my two cut speeds (assuming there are two…)?
Yes. I would set it to the lower of the two speeds so that it comes on for both cuts. The purpose of this speed threshold is to kill the THC when going around tight corners because voltage will rise causing the torch to move toward the plate. If you have your Z speed factor set to 5% you should be ok.
@langmuir-mike Will do. Thanks for the help!
(When you do update the sheetcam post, maybe drop a link to that in this thread in case others have a similar issue)
