Piercing 3/8" thick plate

[RAD]

you guys have any tips for piercing 3/8" thick plate?

I've tried some 3/4" dia. holes any found sometimes the torch tip would colide with the molten metal when indexing from pierce to cut height. I was thinking maybe I should set up pierce points at the center of the hole using the drilling operation, I would pierce remove the pierce slag and edge start the cut..?

I was using 50 amps with 45amp consumables, hypertherm.

[motoguy]

what software are you using? If using Sheetcam, Les created a "pierce only" post that will allow you to pierce all the holes first, clean the pile away, then cut the part.

[KIDTech]

Is it common practice to run higher amps than the consumable is etched for? I was under the impression I read somewhere on the forum to never exceed the amps markings so if it is a 45 amp consumable then you are fine 45 or less but not over 45.

[SeanP]

I used to get that problem cutting base plates a lot, now I use a covering of 'Duck oil' over the whole sheet before starting it really cuts down on that slag pile, not sure if it's available over there or if there is an alternative, it works though.
The pierce only post sounds like it might be well worth a shot as well, I'll have a look myself for that right now

[gary42095]

i use nozzle kleen spray for mig welding on both the torch, and the plate on thicker materials. make the leadin as long as possible and make sure shield has no slag blocking holes inside and out. just my $.02

[SeanP]

Trouble is some of those are water based and get washed off with water table, good point about leadins, start at centre of those size holes.
Just found the link to the pierce only post for sheetcam, took me a while so I'll add it here.
http://www.forum.sheetcam.com/viewtopic.php?t=7059

[RAD]

Thanks guys, yes im using sheetcam. I am somewhat familiar with the drilling operation for piercing holes, I did a dry run once and it seems to work well.

As for running above the rated amperage, my duramax manual specifies using 50 amps for 3/8" thick but illustrates 45 amp consumables, even for 55 amps they show the 45 amp consumables.

I would see if I can locate that duck oil over here that would make life easy by saving time

[WyoGreen]

RAD,
I think this is what Sean was talking about.

http://www.swarfega.com/workplace/products/sdo5l

[acourtjester]

eBay has it but your looking at about $85. for 5 litre and a month delivery time?
http://www.ebay.com/itm/Duck-Oil-5-Litr ... Sw3mpXDbtX

[Brand X]

Thanks guys, yes im using sheetcam. I am somewhat familiar with the drilling operation for piercing holes, I did a dry run once and it seems to work well.

This is a drill operation for the start of your Lead-in on any shape, not just drilling holes..I found using my Victor, solves all those .060 cut height issues..

[tnbndr]

This has me curious. If you pre-pierce and then go back to cut starting at the pierce point won't the torch just start and flame out as it doesn't find any material?

[RAD]

This has me curious. If you pre-pierce and then go back to cut starting at the pierce point won't the torch just start and flame out as it doesn't find any material?

by using a perpendicular leadin that starts just on the edge of the pierce hole might work..?

[jimcolt]

You should be able to pierce 3/8" all day without colliding with the pierce slag pile. My guess would be that your torch is staying in the pierce location too long (pierce delay time too long?) and the height control is activating too quickly.

Here are a few suggestions:

1. Slow down your z axis speed....so it does not move down so quickly.
2. Use a slightly higher pierce height....the book spec for 3/8" is .15", you can go as high as .22" with good results.
3. Check you height control (AVC) delay, perhaps it can be a longer time period or distance before the Arc Voltage Control activates.
4. Watch your piercing carefully, the moment the sparks exit the bottom of the material the x and y movement should begin, and at that same time the z axis should index from pierce height to cut height. Decrease the pierce delay time if necessary.
5. The 45 amp shielded consumables can pierce up through 1/2" very nicely if you pay attention to all of the above. The delay times in the operators manual work...but only if your cnc setup starts the timing based on the arc transfer output from the Hypertherm unit (contact closure on pins 12 and 14 at the CPC port). Some systems do not sense this, or you may not have the function active in the software.
6. I don't recommend exceeding the rated current on a nozzle......that will rapidly erode the nozzle orifice with no other real advantage.


Jim Colt Hypertherm

you guys have any tips for piercing 3/8" thick plate?

I've tried some 3/4" dia. holes any found sometimes the torch tip would colide with the molten metal when indexing from pierce to cut height. I was thinking maybe I should set up pierce points at the center of the hole using the drilling operation, I would pierce remove the pierce slag and edge start the cut..?

I was using 50 amps with 45amp consumables, hypertherm.

[RAD]

Thanks Jim I am going to give those a try. I didn't think about the delay setting being too long

[Brand X]

This has me curious. If you pre-pierce and then go back to cut starting at the pierce point won't the torch just start and flame out as it doesn't find any material?

No, because it's just like edge starting, and will pick up the edge, and move real quickly. Holes that are plasma punched will have a narrower bottom, and the arc will catch that at some point. This process is for cheating the systems max pierce thickness a bit, by using other consumables then the cutting ones.You also can start much closer to actual cut height, so the arc will transfer even easier to the plate after it's plasma drilled.

[acourtjester]

If you did not see this like me here is the extra button Les talked about in Sean's post above.

prepost.jpg (42.69 KiB) Viewed 3247 times

prepost.jpg (42.69 KiB) Viewed 3247 times

[motoguy]

That button only exists/works/shows up in the DEV version, I believe. Still have to manually change the machine post in the stable version.

[kkroger]

On thicker material 3/8 and up I use a "Wiggle" pierce. and as long as is feasible lengthwise. for instance a half inch hole in 3/8 plate I will use an ARC lead in and then wiggle and make the lead and wiggle about .375 so the torch is not just sitting there. I cut AR500 plate 3/8 and Half, Mild Steel Plate up to 5/8" with my pm65 using a wiggle lead in.

[motoguy]

kkroger, what controller and thc software/setup do you use?

[SeanP]

kkroger, what controller and thc software/setup do you use?

It's a pity you can't use a slower feed rate with wiggle pierce, it shakes the hell out of mine when I tried it.

[kkroger]

kkroger, what controller and thc software/setup do you use?

CandCNC Ethercut 620-4... DTHCIV...
No mystery... I've been too busy to post here for about a year or so! LOL!
Mine doesn't shake or shimmy it just runs the arc I set for it and then begins cutting...
You can also use Pam Cooking spray as "Anti Spatter" or you can use Talcum powder....
Or any number of other things...

I run Sheetcam for the CAM portion of my work, and I use Mach3 for my control software, and any number of available CAD and Design software...

[Brand X]

kkroger, what controller and thc software/setup do you use?

It's a pity you can't use a slower feed rate with wiggle pierce, it shakes the hell out of mine when I tried it.

It's not recommended by Hypertherm anyway.. I have been trying to get Les to make a program to raise the torch after firing the arc. to a higher level, then come back to cut height, and move.. Like the big boys do it.. So a setting of Initial Height. (Fires there like a standard pierce height) Then a Pierce height that is higher then normal, then cutting height. Just like my Modern Esab PT-37 Machine torch specs give me.. I did get Les to make a post to for Plasma drill at the start of the Lead-in, so I think it's your guys turn to see if you can get some movement there.


I still see little reason for anything other then factory setting on my Hyperthem/Esab, or Victor plasma cutters for a 3/8 pierce.

[motoguy]

kkroger, what controller and thc software/setup do you use?

CandCNC Ethercut 620-4... DTHCIV...
No mystery... I've been too busy to post here for about a year or so! LOL!
Mine doesn't shake or shimmy it just runs the arc I set for it and then begins cutting...
You can also use Pam Cooking spray as "Anti Spatter" or you can use Talcum powder....
Or any number of other things...

I run Sheetcam for the CAM portion of my work, and I use Mach3 for my control software, and any number of available CAD and Design software...

I couldn't remember what you used. I seem to recall Tom saying that wiggle pierce doesn't play well with the CandCNC controls. Sounds like, in your case anyway, that's not the case.

[tnbndr]

I seem to recall Tom saying that wiggle pierce doesn't play well with the CandCNC controls.

I tried the wiggle pierce with my PM45 on some 1/2" plate I needed to cut for someone and it worked well. Have not had to use it since.

[jimcolt]

The Powermax45 and 45 XP are both rated for straight in piercing up to 1/2" steel, when you follow book specs (pierce height, pierce delay time)...you will get a minimum of 300 pierces in 1/2" at the rated pierce thickness if you 100% follow the book specs, wiggle pierce is not recommended or needed.

The same is true for the larger Hypertherm systems with ratings of 5/8" pierce for the Powermax65, 3/4" pierce for the 85 and 7/8" pierce for the 105 systems. The design of these torches and shielded consumables was well tested before we ever shipped the first units. There really is no reason to experiment with special pierce techniques unless you need to exceed the factory rated pierce thickness ratings. I have done 1" steel on a few occasions with a straight in pierce with my Powermax85 by simply increasing both the pierce height and the pierce delay times as well as reducing the z axis speed (so the torch does not hit the pierce slag pile when transitioning from pierce height to cut height). Jim Colt Hypertherm