THC Codes upset corners???

In preparation for fitting a THC unit, I thought I’d try adding the M101/M102 codes to my post.

I have a test job, a 50mm square that has loops on the corners to keep nice sharp corners, however with the M codes added, when I dry-run this code in Mach it runs to a corner, stops, cuts the loop, stops, cuts the next edge then repeats on all corners??

Is there a reason it does this or is Mach not set correctly, surely just adding THC on/off codes should not upset the smoothness of the code?

Unfortunately, running a macro in MACH (M101, etc) will cause a pause. You need to have a newer system like CandCNC offers with their DTHC II or IV that moves the height control out of MACH and into the hardware. What THC system are you planning on getting?

I’ve ordered a Proma unit, it’s basic but seems to function ok in the YouTube videos on it.

Not sure what happens if you don’t use the macros ?

Never used one before.

What is the reason?

If it does not work, I guess it will just have to live on the built-in start delay and any thing Mach can throw at it ?

I believe it’s just a “fault” ( if you want to call it that) of MACH. You could still use the macro before and after “holes” to allow a change of speed, just not mid cut.

Hmm, ok, thanks.

Any idea if Mach ignores thc signals on small circles or lead-ins etc??

I’m just trying to figure out how this all plays together.

That would be a function of SheetCAM and the new “rules” system to turn on / off THC and slow down. That feature is available in the development version and should be in the soon to be released version “6”.

So if Mach can’t handle the THC on/off without stalling, this feature wont work anyway?

Heading over to the Mach forum to see how this will work…


I have downloaded the test version but as I said, if mach can’t handle macros without stalling, it’s all in vain surely?

The overcut feature looks promising though:)

Not getting answers from the mach forum either?

There are the S10/S20 codes to turn thc on/off, depending if your hardware/software is fairly recent.(Check DCC on the candcnc website)
These do not stop motion.
I havent tried them yet, still need to update my mch screen.
Also, if you need to stop the torch and continue motion(like finishing a hole)
try the M10P1 code. It stops the torch without a jerk in motion.

No, need, just discovered this…

mach 3 does have what it takes, it’s a setting called anti-dive, it takes a % figure you enter of the feedrate below which it turns off the THC signals to the z axis. So on small circles cut at say 70% normal, if set to 80% THC would be off -sounds just like what it needs.

Corner deceleration would also stop THC action.


Youre almost right.
Anti dive locks thc ON CORNERS when it gets below the preset speed ex:70%

But, if you program a speed change in sheetcam, that speed becomes your preset speed.
Running with anti-dive at 70%,
If you run at 200 ipm, anti-dive will kick in at 140 ipm.
But, if in sheetcam you slow down corners to 50%, mach3 will see 100ipm as the “normal” speed and will not lock thc. and will drive the torch down.

Ooh, that’s a good point, thanks.

Gets a bit complicated doesn’t it :slight_smile:

I’m sure sheetcam will reduce speed on circles etc so this only seems to be a partial fix.

Will have to look at the code.

Nothing is ever easy :wink:

Anyone got suggestions?

As i said, i still have to try the S codes.
But you can use the M codes on holes using the cutting rules.
In rules editor;
On small circles, smaller than…
start code: put your thc off code
end code: put your thc on code.
This will automatically turn off thc on small holes, run the hole at the speed you want, then turn thc back on after the hole…no need to put it on a different layer.

That’s good stuff,I can see these new rules coming in handy :slight_smile:

Will need to have a play with it.

Just a thought…

If we now have the excellent new rules system where I can choose to reduce speed for say a 30mm circle, is it best to now modify the POST file to remove the “slowdown on circles <xx dia” entry, maybe set it to 1mm or something like that.

reasoning was that if this was not done we would have two slowdown rules running - cutting rules plus POST rules??

If im not mistaken, sheetcam will always take the lowest feedrate between 2 overlapping rules.

Ok thanks, but to stop confusion or doubt, would it be a reasonable idea to disable the POST slowdown entry if we are using rules?

The post does not know about rules and vice-versa. It is a good idea to disable slowdown in the post if you are using rules.