blow holes in plasma cutting

I am trying to plasma cut some art work. I want to cut just a single line (like to highlight a feather on an eagle drawing).
When I cut the line I get a blow hole when the torch first starts. I have tried various combinations of settings, but without success. Could anyone suggest how to set up for this cut. I have a LDR Motion Systems table, Hypertherm 65, SheetCAM and Mach3 software.
Thanks for any help

Robert Grams
72686 331 Ave
Imperial, NE 69033
308-882-4084 home
308-883-8000 cell

This email has been checked for viruses by Avast antivirus software.

You can’t completely eradicate the blow hole. About the best you can do is use a very short pierce and then use a cutting rule to slow down the beginning of the cut. You will have to experiment quite a bit to find the best settings.

When you say a very short pierce, I assume you mean a short pierce delay. If that is the case I am already using “zero” for pierce delay. What else can I do here?

What do you mean when you say to “use a cutting rule to slow down the beginning of the cut”? And how do you do this.

Thanks again for your prompt reply.


I’m trying to do pretty much the same thing, plasma does have drawbacks, one of them being that the pierce is always bigger than the cutting kerf.

I think Les is hinting at slowing down the start of the cut so it makes the kerf wider - the torch is moving too slow for a normal cut so it burns away the metal from either side.

I have not tried this myself yet but it sounds possible, maybe.

I try to keep the flow for open cut lines to start at the same end so all the pierce holes are the same, or try to build them into the design.

There may be other ideas but I know exactly what you mean and it’s a pain.

If your pierce delay is zero already there isn’t much else I can think of. Try reducing the pierce height to nearly the cut height. That will reduce the pierce time further.

If you are using Mach3 go to ports and pins and check your spindle setup. the spin up and pin down delays should all be 0.

I was playing with this morning, tried deliberately slow cutting, pierce was on zero anyway. There seems no way out of the hole, I was getting a 0.85 kerf but the pierce was maybe 1.6mm or more, it’s pretty noticeable.

I guess if I was really worried I could flash the holes with Mig or Tig but hopefully won’t need it.

I will try the low pierce height and see if that makes a difference .

Is there a way to get sheetcam to do a reverse pierce at the end of an open line cut??

That would give at least a matching hole at each end of a cut, could possibly work with that on some designs.

Or a better way???

I haven’t tried it,but you would think adding a time in ‘pause at end of cut’ in the tool would do that ok.

Have you got the max acceleration out of your z motor as well, that might shave some off.

If it’s thin material I have seen it mentioned about using same pierce height as cut height.

The pause at end is after the torch is off, it allows the flame to go out fully before moving.

I guess one way would simply be to paste in a P0.5 line before the M05/torch off line.?

My material is mostly 3mm steel, I am going to try piercing at cut height and see if that makes any difference.

Thanks Dave, I didn’t realise that.

The pause at end is after the torch is off, it allows the flame to go out fully before moving

I imagine the post could be modified to use the “Pause at the end of cut” to occur before the torch-off command. If I had many to do, I would try this.


Could also modify the artwork to have a point at one end of the line, use the torch as a drill on the point then start the cut at the opposite end and cut towards the “drill” hole?

The POST option sounds good too but a better refinement would be to have a check-box in the tool list for “Pierce at both ends” but I guess that’s leaning towards a custom program modification?

The check-box would be nice.

If it could be incorporated, should the check-box be available in the Operation instead. I could see a layer for these “both end pierce” or “Pause at end of cut” and then other layer(s) for profile, etc. using the same “tool”. The option in the Operation may be more intuitive (at least in my mind).


I think either would be good.

I was just presuming of course that merely pausing for say 0.5s at the end of a cut would create a similar effect to a pierce.

Sounds good though.

To make the end delay work the other way around it only takes a small tweak to the post. Edit your post and look for function OnPenUp(). Depending on the exact post the code may vary a bit but you’ll probably have spomething similar to this:

   post.Text (" M05\n")
   if (endDelay > 0) then
      post.Text (" G04 P")
      post.Number (endDelay,"0.###")

Change it to:

   if (endDelay > 0) then
      post.Text (" G04 P")
      post.Number (endDelay,"0.###")
   post.Text (" M05\n")

Sounds good, thanks Les

however, as i already use the “normal” end delay it could get a bit messy :slight_smile:

How far into the realms of dreamland would it be to get the check-box added to the cut screen as an option “Pierce both ends”???

I don’t really see that it will work very well and this is a pretty unusual request so I’m afraid I probably won’t add it.

Try manually adding a delay to the g-code before it turns the torch off. If that gives you the effect you want I’ll explain how to tweak the post to add an extra parameter to the tool definition for a pre torch off delay.

That sounds just as good, thanks for that Les.

I will test it as soon as possible and report back.


Well, I did have a mess-about tonight, I tried pausing for a second at the end of the cut, had surprisingly little effect really, very slight hole but nothing like a pierce.

Then I tried a reverse pierce - make the cut, then keep the torch on at the end and lift back to pierce height before stopping the torch. This gave a reasonable effect but was still smaller than the start pierce.

Piercing at cut height made very little difference and would likely be bad for the consumables.

The final test was a full pierce - move to the end of the cut, make a pierce, drop to cut height and stop the torch, lift back up. Then move back to the start and cut towards the pierce hole. This gave perfect results as expected - a line with a matching pierce at each end.

So, the question is, can the POST be modded to make a pierce at the end location first ???

The only other way is to mark one end of all open cuts in the CAD stage then “drill” these with the plasma as a first op.

Unfortunately the post doesn’t know where the end of the cut is until it gets there. It would not be able to pierce the ends first.