CNC Plasma Hole Cutting: Best Practices

[jimcolt]

Thought I'd post this as it probably is the most often asked question regarding cut quality with CNC and an air plasma cutter. This is a dirct question from my personal email from a day ago, and my rather lengthy answer. Feel free to contribute or ask further questions! Jim

Questions:
I have recently purchased a cnc plasma machine with a Hypertherm Powermax 125. I’ve read many articles and posts you've written about achieving better hole quality. I am cutting 5/8" plate and trying to cut 3/4" holes. You stated in an article that I should be using the 65amp consumables. Can I turn up my amperage without destroying my consumables? I am very new to the cnc plasma so this is quite the learning process
Can you recommended a machine set up for this plate and hole size?
Thanks for your time.

Jim’s Answer:
Hole cutting on most cnc machine requires a bit of technique once the hole diameters become smaller than about 1-1/4”. An air plasma arc will tail back (bottom of the cut trails behind the top) a bit when you are cutting at the ideal speed for outside plate contours (minimal dross and angularity). This tail in the arc will increase angularity as the hole diameter gets smaller…..so here I will list some of the best practices that will improve overall hole quality on thinner materials. Good quality small diameter holes are a coordinated function between the part design (lead ins, lead outs, etc.), the capability of the plasma torch and consumables, height control settings as well as the cnc machines ability to stay on path at the desired cut speed. On our high definition class plasma systems 100% of the hole cutting technique can be automated when paired up with specifically designed cnc machines (True Hole technology), however the lower cost air plasma’s and the cnc machines they are typically used with do not have this ability. So, to get the best holes:

Rules of thumb for best holes under 1-1/4” diameter

- Always choose the lowest amperage process from your Powermax cut charts that will have the ability to pierce the material and thickness you need to cut. On your Powermax125 your cut charts indicate that you can pierce 5/8” steel with the 125 Amp, 105 Amp and 65 Amp processes. The 65 amp process will produce the best hole quality. The 105 Amp process will produce better hole quality as compared to the 125 Amp. The primary reason that the lower amp processes work better is because the machine speeds stay lower allowing the torch height control and the motion control to react well with the characteristics of the plasma arc.

- If you use the 65 amp process on 5/8” you will see that the book specs for best cut quality are: Pierce height (critical) .24”, Pierce delay 2 seconds, cut speed 23 IPM, cut height .06”. Using these specs exactly will get you best cut quality using the 65 amp shielded consumables at 65 amps. Increasing the amperage will rapidly wear the consumable parts, and is not recommended.

- Design your hole with the start point near the center. This will allow the height control to 1. Find the surface and retract to the correct pierce height (.24” on 5/8”), 2. Allow no movement (x, y or z) until the pierce time (2 seconds on 5/8”) is complete and the arc has fully penetrated the material, 3. The long lead in to the hole allows time for the height control to index the torch from pierce height to cut height….which must be done before the torch reaches the radius contour of the hole. The long lead in also allows the torch air pressure to stabilize.

- The lead in design is based on your machines acceleration capability and mechanical tightness. Machines with low acceleration rates and mechanical backlash tend to make better holes with a radial lead in shape. Tight machines with excellent acceleration (in the .3G range) will make better holes with a straight lead in. Starting near the center with the lead in also allows the slag pile (pile of metal on top of the plate around the pierce hole) from interfering with the arc during the hole contour. If the arc runs over top slag it will deflect, and the deflection is usually noticed on the bottom of the hole as a “divot” in the hole shape.

- Best practice for holes under 1-1/4” diameter is to program the speed at approx.. 60% of the suggested best quality speed for the material being cut. The suggested best speed on 5/8” steel at 65 amps is 23 IPM, so program all holes under 1-1/4” to cut at about 14 IPM. This lower speed will produce some (easy to remove) dross on the bottom, but will reduce the amount of taper in the hole.

- Design your hole program to use an overburn at the end of the hole, do not use a lead out into the center slug as this will create an anomaly in the shape of the hole as well as shorten the plasma consumable parts life. An overburn is simply staying on the hole radius past the lead in point by about .150” to .200”. If your cnc control and CAM software have the ability…it is best to extinguish the plasma right at the 360 degree lead in kerf crossing, yet continue the motion on the hole radius for the .150” to .200” distance. The plasma arc takes a few milliseconds to fully extinguish, and this technique, if it can be done, will smooth the transition between the lead in and the end of the cut.

I can provide a .pdf file that outlines much of the above info….it should help (contact me via email). These techniques will improve your hole cutting at all power levels, however I stand by my statement that the best holes will be done at the lowest power level that we can pierce your material at. While all of the above is fully automated in our High Definition class systems (assuming they are integrated to a cnc , height control and CAM software with the capability for True Hole technology), once you develop the best specs for each material thickness it should be an easily repeatable process for you.

If you have questions feel free to contact me! Jim.colt@hypertherm.com

Best regards, Jim Colt

[davek0974]

Interesting stuff.

Does the 1-1/4" hole slow-down apply to the smaller capacity machines too - like the PM45??

I'll be playing with overburn etc as soon as i have my new table up and running, the existing one always left a divot at the end of the cut regardless of settings.

[see&see]

From another Jim Colt article: "The energy density of a Hypertherm 45 amp nozzle running at 45 amps is the same as an 85 amp nozzle running at 85 amps, roughly 12,000 amps per square inch."

I'm using my PM85 with the mechanical torch at 45 amps most of the time up to 1/2" plate and getting better quality cuts and holes. The trade off is you cut slower. 1/2" plate at 20 ipm and 3/8" at 32 ipm. Slower on holes and I'm actually getting less bevel than I had using the faster 65 amp process.

Also, go figure, since adding a desiccant and carbon filter following my refrigerated dryer I'm getting better cut quality at 45 amps and longer consumable life..

[davek0974]

Very interesting, thanks

Also note the point about adding a desiccant after the dryer, I have a dryer and thought that was it, maybe not.

[see&see]

I had my moisture problem solved also, I thought. The fan cooled condenser and refrigerated dryer are directly receiving hot air from the compressor head. They do the job and work well as my compressor tank is bone dry. I haven't found a drop of moisture in the tank since I added the condenser and dryer.

This summer our normal 20% humidity in the West has averaged over 50%. I'll post a picture of my desiccant dryer later today. The blue beads on the bottom of the dryer bowl have suddenly turned orange in just under 30 minutes of cut time..

[beefy]

I added a 4 foot LPG tank straight after the compressor and buried it vertically in the ground where it's nice and cool, even in summer. Works great as an initial condenser. Plumbed in a tiny line from the bottom of the tank and into the shop. It's amazing just how much water I bleed out there. After the tank the air goes to a refrigerated air dryer, and finally to a dessicant filter.

Tried the old blowing air on a mirror and never get any signs of moisture.

[davek0974]

My compressor feeds into a tank and then to the dryer via about 10' of hose, the drain valve on the drier hardly ever goes off but i do get a fair bit from the compressor tank.

Might look into a desiccant but i'll try the mirror test first

[jimcolt]

Dave, slowing down works for all plasma cutters on holes. It is more important on smaller diameters, that is why I use 1-1/4" and below diameters in my "rule of thumb".

More advance CAM software and cnc controls will automatically recognize hole diameters in the CAD drawing and apply proper cut speeds and lead-in, overburn specs for the particular hole size, material thickness and power levels. Holes then are always good.

My post about holes makes the assumption that we are using minimal (low cost) software and minimal cnc (low cost)......and we do not have an expensive CAM and CNC setup. In industrial applications where you cannot afford to waste time experimenting....expensive solutions are the best decision if it keeps the machine running and minimizes the operator from having to tweak every cutting operation.

Industrial applications want material on the table, push the start button, remove parts and scrap....then repeat.

Jim Colt

Interesting stuff.

Does the 1-1/4" hole slow-down apply to the smaller capacity machines too - like the PM45??

I'll be playing with overburn etc as soon as i have my new table up and running, the existing one always left a divot at the end of the cut regardless of settings.

[jimcolt]

see&see,

I too use my Powermax85 (on a Plasmacam) at 45 amps up through 3/8", (rarely on 1/2") for best cut quality....especially if I need holes t hat do not need re-drilling/reaming. Low power, low speed are the keys to best edge quality / angularity. At low power on heavier materials you have to pay careful attention to your piercing technique.

Your comments about moisture control are spot on, however keep in mind that moisture is regional and seasonal! I only use my refrigerated dryer during the 8 or so summer weeks of high humidity here in NH. The rest of the time the air goes directly to all of my Hypertherm plasma's, no additional filtration whatsoever.

Another thing about moisture and how it affects plasma cutting......some plasma cutters are very, very affected by small amounts of moisture and consumables will wear very fast. Hypertherm has been quietly designing torches and consumables to survive with small amounts of moisture for the last 10 years or so. While we recommend clean, dry air......if you do get moisture with the newer Hypertherm units it will have a minimal effect on consumable life and cut quality as compared to other plasmas and even older technology Hypertherm's.

Jim Colt

From another Jim Colt article: "The energy density of a Hypertherm 45 amp nozzle running at 45 amps is the same as an 85 amp nozzle running at 85 amps, roughly 12,000 amps per square inch."

I'm using my PM85 with the mechanical torch at 45 amps most of the time up to 1/2" plate and getting better quality cuts and holes. The trade off is you cut slower. 1/2" plate at 20 ipm and 3/8" at 32 ipm. Slower on holes and I'm actually getting less bevel than I had using the faster 65 amp process.

Also, go figure, since adding a desiccant and carbon filter following my refrigerated dryer I'm getting better cut quality at 45 amps and longer consumable life..

[davek0974]

great, thanks Jim.


When you say low power and slow for good small holes, is it worth going below 45A?

Or is the PM45 tuned for best quality at 45A (assuming use of standard consumables)?

Just wondering

[jimcolt]

Dave, reducing the amperage to less than the design amperage of a particular nozzle reduces the energy density of the arc. Lower energy density means a softer arc which will have a tendency to cut with varying angularity and more dross. I always recommend (if your machine has good acceleration and speed characteristics) running at the max rated amperage of the consumables, and using the lowest power rated consumables for the material and thickness. Max energy density works best.

Machines that cannot cut at the desired speed on fine features and small holes simply will not cut as well as machines that can maintain speeds. Changing the physics of the plasma arc by reducing energy density will not solve the problem, although you may find a happy medium that works for your machine and is acceptable.

Our engineering team is looking at lower powered consumables that will likely help produce better cut quality on machines with lower acceleration rates.

Jim

[davek0974]

Thanks, that makes sense, hopefully the new table will allow me to run at book specs at last

[whiskeymike]

Thought I'd post this as it probably is the most often asked question regarding cut quality with CNC and an air plasma cutter. This is a dirct question from my personal email from a day ago, and my rather lengthy answer. Feel free to contribute or ask further questions! Jim


Best regards, Jim Colt

Jim, this is a great write up. I've used it a great deal over the past couple weeks in improving my hole cuts and it's helped. A followup question for you. I assume this references circular/round holes. Would you change anything for making it a hexagon hole? I'm looking to make some holes in a piece where I'll drop a flanged nut into and weld it in. I'll try some cuts tonight and see how close I can get it.

[jimcolt]

holes like square and hexagon are tougher in most cases than round holes. You likely will need a straight lead in, and acceleration must be as high as your machine can go without getting shaky.

Jim Colt