Plasma drill

Hi Les,
Just a question about Plasma drill. Is there a way to setup a plasma drill to punch through at all the start points on a cut piece? Just at the lead-in point of every pierce. The reason I am asking this so you could pre-pierce with a drill program on thick metal, and then change to a new nozzle and run the program to cut out everything in another layer using a standard plasma tool. Of course starting at all your pre- plasma drilled holes… It would allow better overall cut quality because there would be way less chance of wiping out a shield or nozzle. It’s similar to edge starting on thicker materiel, and would add capability to your overall piercing thickness…

Many times using the lowest amp nozzles that will cut though the steel, yields a much better cut overall.Generally have to go up too much on amps and nozzle size to get it to Pierce clean enough, but edge angularity suffers, along with cut face quality… Just trying to cheat the system a bit…


That can only be done by using two post processors. The first post would just generate the pierce holes then the second post would generate the cut paths as normal. I would have to make a post to do the drilling.

I was wondering about this very thing as well.

I am using the MP3000 DTHCII+Scriber2 post (as many are) in case you needed one to try it out on… :)Since I am on this subject,thought I would add this below…

I am guessing I could now use with the plasma drill parameters set like this below. My Esab cutter had a setting for starting a Pierce at a lower height, and moving up to a higher pierce height while finishing the pierce on thicker metal. I would think just swapping the pierce height, and cut Height parameters in the drill tool setting would make this possible? As long as you had the refDistance set to zero . It would allow for longer life of your sacrificial piercing consumables… So you are still using the original pierce height, and when it moved to cut height, it would move up instead of down… I don’t see any reason the z would not move that way too… I need to go down to the shop, and run it a bit…

Initial Pierce height Pierce Height
.200 0.280

OK tried the different heights while piercing, The torch moves up, but only after the delay time has expired, To truly make it work correct, it would need to move up at the time it fires/arc transfers to the plate… I had to manually edit thc S20 code to S-10 to keep the THC off. No need for it anyway in the pierce mode…Just can cause issues, Made a bunch of drills in 750. ms, and all is good… 80 amp Victor is rated for 5/8 pierce, and this moves it up to .750 and maybe a bit beyond that too…Need to get the torch to lift correct,to get any more… The victor can cut .750 really nice at 60 amps output, slow but extremely nice finish. So drill @80 amps, and cut at 70/60 amps is a nice option…(have nozzles for each size) Wish I still had my A-120 now…:slight_smile:


I have attached a post that should do the piercing. You will have to use a different post for cutting. If you go to Options->plugin options->moreposts you can add extra post processor buttons so you don’t need to go through Options->machine->post processor each time.
Mach3 THC pre-pierce.scpost (3.35 KB)

Love this! Had to babysit a 1/2" sheet earlier this week, making sure the torch didn’t end up in the slag pile as it moved out of the pierce. Looking forward to trying it out! Thanks!

Exactly what I was looking for! Once again Thank You Les!! :smiley:

Are posts interchangeable between Linux and windows versions of Sheetcam?

Yes. There is no difference in the posts.

learn something new nearly every time you look on here.
Will have to give that post a try, could be useful for sheets of base plates.

Thanks for writing this for us

This post is not working in CommandCNC. Giving “unknown G code” errors. I’ll post on the CandCNC forum and see if they can tell me what needs to be changed.

I’ve posted the Mach code in the CandCNC forum, but had no success getting the admin to modify it for CommandCNC use, nor in being told the differences in syntax (so I could modify it myself). I’m planning on digging in manually, and playing with it to see if I can slog my way through a conversion to a working pierce-only post for CommandCNC. I’ve never played with significant post modification, so we’ll see what we can do.

In the meantime, if any of you are familiar with the differences between Mach post syntax and CommandCNC (linux) post syntax, I’d appreciate any tips you may have to offer!

Here’s the Admin response from the CandCNC site:

“Well Les is not correct. There is no real difference in the FUNCTIONS but there is a big difference in Syntax (the actual Gcode commands )”

There is no difference between the Windows and Linux versions of SheetCam but as Tom said there is most definitely a difference between Mach and CommandCNC. I’ll see if I have a CommandCNC post and tweak it to just pierce.

Here is one that was put together (not by me, untested, no guarantee it’ll work) before Tom came in and put a stop to it. He is very adamant that pre-piercing is not the “correct” way to be cutting. All I know, is using the pre-pierce post on Mach (with thick material) saved me a lot of headaches!

I haven’t had a chance to try this one out yet, but you may take a look at it.

THC_pre-pierce_LinuxCNC.scpost (4.23 KB)

What does Tom have against pre-pierce? It makes a lot of sense to me.

Here is what he has to say about it:

“I pointed out that the idea of pre-piercing is not a valid method of doing plasma cutting. The whole pierce process on thick metal is to prevent blowback that kills consumables. For pecking drill spots we have the Peck pierce option that can be used to change the pierce characteristics and just make divots. I have used all the way down to 16 ga without piercing completely through. On thicker material the BEST solution is to have the RS485 serial port on a Hypertherm and use the “Soft Pierce” option in SheetCAM (using our POST) and set a % of the full cut current to start the pierce . It automatically lowers the Z plunge rate too . The concept is to get a more controlled pierce and prevent the consumable killing back splash. Users report they double their consumables life on cutting 1/4” and thicker material."


“Once again this is forcing the plasma to do things that make little sense. Pre-piercing holes does nothing to increase consumable life or improve the cuts. What destroys consumables is piercing no matter when its done. If you did the pierces at one current setting and plunge rate versus the other it MIGHT help, but then again so does having control of the cut current dynamically and altering the pierce process in real time. I am sorry but I cannot release a POST that I then have to support and maintain that is contrary to doing proper plasma cutting. If you want to modify and distribute a Post to do that then please be prepared to support it. My tech team is drilled on the proper methods of cutting and how to get the best results.”

I can see where Tom is coming from. It looks like his system has a way of piercing that reduces the blowback problem, making pre-pierce largely unnecessary.

Once again this is forcing the plasma to do things that make little sense. Pre-piercing holes does nothing to increase consumable life or improve the cuts.

However if you use worn out consumables for piercing it can save your good consumables.

Those are benefits. For me, the largest benefit was the ability to pierce the holes, then remove the slag-pile from the area before proceeding to the cut. Prior to the pierce-only post, the torch often proceeded through the slag pile as it moved along the lead-in. This resulted in a snagged torch tip, and pulling the torch off the mag mount.

It also allows you to pierce beyond recommended thickness, because you’re using already-trashed consumables.

A ramp pierce moves the torch away from the slag pile as well as allowing piercing thicker than rated material. And you don’t have to change consumables.