SheetCam and Mach3 Pierce Delay

This is something that I see has come up several times and it got me in the beginning so I will share what fixed it for me.

First make sure that the “G04 Dwell in ms” is checked in the General Configuration settings in Mach3

Then make sure that the ms is checked in Sheetcam under the “Application options” under the “Units” Tab

Then when editing your tool setting in Sheetcam where it has the pierce delay box for 1/4 sec you will add 250000 I know that there is only 1000ms in a second and it doesn’t make any sense to me but it works. I wonder if someone messed up on a decimal point or if they thought there were a million ms’s in a second?

When you hit enter it will look something like this in the pierce delay box “2.5e5 ms”

Then with it opened up in Mach3 if you scroll down to your G04 code you should see that it has a P250 behind it and as long as your Mach3 software is configured to treat the “04 Dwell in ms” then you should be good to go.

Then you should be good to go on pierces less than 1 second, at least that is how it works for me.

If you need more than 1 second like 1.5 then enter 1500000 and that should give you a 1.5 sec pierce delay.

Hope this helps and works for those that need it.

Safe cutting.

1 Like

I came over from the other post that I hijacked. I am still running into issues with this. I wonder if it is specific to the cutter/Hypertherm 45xp. I can’t get the pierce delay down below 3 seconds, almost 4. no matter what I change it to or what I’ve done. I wonder if there is a setting for the pre-flow of air?

It may be, I don’t have that cutter I have a primeweld and there isn’t a preflow that I remember, have you cut with it before with less delay?

no it has been like this since the beginning. I just checked - no pre-flow. I mean the cutting part of it isn’t bad, but the pierce holes are pretty big and noticeable and I wonder if it’s because it is sitting there for almost 4 seconds. I have changed the other pierce delays in the .tap file to see if that would make a difference. No matter what I do it always delays that long.

I love the way this thing cuts. I just can’t figure out why I can’t edit the delay. One of the reasons I purchased this cutter after buying an Everlast was the cut quality - now to see that the pierce delay, on my end, isn’t configurable.

What post processor did you select for sheetcam, it sounds like it may be waiting for the z axis to travel down I am fixing to leave work and it takes me about an hour and a half to get home then I will look and see what post processor I chose, I believe there is one for mach3 with no z axis and I may have chosen that one but it has been a while and I already packed up my laptop I am also sending you a pm.

1 Like

Not sure if you’re still on here trying this tonight or not but I just got home and checked the software and this is what I have chosen for the post processor in sheetcam.

Are you using the crossfire profile when starting mach3 ?



Are you using the crossfire profile when starting mach3 ?

Not sure which one of us your question is directed to but yes, I am using the crossfire profile with Mach3

Gunny, download this file and change the .dxf to .tap then load it in your mach3, it is a simple square 6x6 with 5 lines, I use it for finding the correct speed and setting for new steel. I currently have it set for the following
Line 1 = .1 sec pierce at 100 imp
Line 2 = .2 sec pierce at 120 imp
Line 3 = .3 sec pierce at 140 imp
Line 4 = .4 sec pierce at 160 imp
Line 5 = .5 sec pierce at 180 imp
Outside cut = .9 sec pierce at 200 imp
Then it should return back to 0-0 and rewind the gcode.
You should see a slightly longer delay in each line with the longest delay on the outside.

Line Test.dxf (1.4 KB)


yes, I am using the crossfire profile when starting mach3

Ok so I used the post-processor that Donald suggested and IT WORKED!!! I have a 600ms or .6 second delay on my pierce and it worked perfectly. I am going to use the file that Donald posted/sent so I can just test and watch some of the pierces, so I can get a good idea of what I want to use on the metal I’m using most of the time - 16gauge.

I almost want to hook up the Everlast and see how she runs.

My only question is where did this come from? Was it something I did, most assuredly?

Anyways, I feel like now I just went and upgraded everything.

Thank you guys for the patience and trouble-shooting.


Glad that I help. The everlast may do just fine. I believe that the post processor with the z axis commands were throwing your times off.

Safe cutting.

1 Like

It’s a game changer for me. These were at 45amps with fine cut consumables on 16ga CRS.

image image


Those look awesome, makes me think that maybe I need to go with the hypertherm? I’ve got my Primeweld 60 cutting cutting good but nothing like that on the backside.

now you can breakout your feeler gauges and see how wide your gap is on the one that you decide to use and enter that in sheetcam then you will have the kerf set properly.

Happy cutting.

Continuing the discussion from SheetCam and Mach3 Pierce Delay:

what are your setting for 16 gauge on the primeweld 60? I cut a piece out yesterday using the setting below but left alot of dross in the backside…

.9 tip
28 amp
50 psi
130 ipm

Don’t have any 16g material because my friend’s wife works at a fab shop that had 7000lbs of 18g material in 19.5 X 30.5 inchs, for twenty cents a pound so guess what I’ve been cutting.

Here is the cut sample that I settled on the other day and I really think that it is pushing it a little and I have slowed down to 220 ipm since then and it is cutting good for what I am cutting.

Maybe you can get a little more speed and air and the back will get better?

yeah your lines are pretty clean compared to mine. I was going pretty much the book setting. i would think raising the air pressure would make it worse.

Mine actually got better with more air, you can also take your swirl ring out and flip it over and see if that makes a difference, they are directional and it can make a difference. Mechanic on this forum has allot of info about the consumables and what you need.

I forgot to tell you that I am using a 40 amp shield and they came from Mechanic, I haven’t tried any of the fleabay tips but as long as his are working then I’ll keep going back to him.

I’ll see if I can get some 16g later and see what I can come up with but not sure when that will happen.

1 Like

i’ll try upping the air and speed. i though 130 was already fast enough… lol

I’m also using the 40 amp tip (.9). I bought some from gamblegarage.