blow holes in plasma cutting

tumbleweed · Post by **tumbleweed** » Wed Feb 11, 2015 4:52 pm

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.
www.avast.com

Post by **Les Newell** » Wed Feb 11, 2015 5:06 pm

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.

tumbleweed · Post by **tumbleweed** » Thu Feb 12, 2015 4:40 pm

Les
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.

Tumbleweed

Davek0974 · Post by **Davek0974** » Fri Feb 13, 2015 3:08 pm

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.

Post by **Les Newell** » Sat Feb 14, 2015 3:15 pm

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.

Davek0974 · Post by **Davek0974** » Sun Feb 15, 2015 3:17 pm

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 .

Davek0974 · Post by **Davek0974** » Wed Feb 18, 2015 7:48 am

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????

SeanP · Post by **SeanP** » Wed Feb 18, 2015 8:47 am

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.

Davek0974 · Post by **Davek0974** » Wed Feb 18, 2015 9:06 am

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.

SeanP · Post by **SeanP** » Wed Feb 18, 2015 9:13 am

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

PK · Post by PK » Wed Feb 18, 2015 10:49 am

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.

Paul

SeanP wrote: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

Davek0974 · Post by **Davek0974** » Wed Feb 18, 2015 11:40 am

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?

PK · Post by PK » Wed Feb 18, 2015 12:35 pm

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).

Paul

Davek0974 · Post by **Davek0974** » Wed Feb 18, 2015 1:17 pm

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.

Post by **Les Newell** » Wed Feb 18, 2015 1:34 pm

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:

Code: Select all

   post.Text &#40;" M05\n"&#41;
   if &#40;endDelay > 0&#41; then
      post.Text &#40;" G04 P"&#41;
      post.Number &#40;endDelay,"0.###"&#41;
      post.Eol&#40;&#41;
   end

Change it to:

Code: Select all

   if &#40;endDelay > 0&#41; then
      post.Text &#40;" G04 P"&#41;
      post.Number &#40;endDelay,"0.###"&#41;
      post.Eol&#40;&#41;
   end
   post.Text &#40;" M05\n"&#41;