[jimcolt]

The question about cutting good quality bolt holes comes up often....and in fact just yesterday I received this typical question (below) from a new machine owner. I thought I would share the question and my long answer as it will likely help others improve their processes. 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

[johnnyg]

Jim,

Thanks for taking the time to write great posts on this forum and others. I appreciate your knowledge on all things cutting! Keep 'em coming.

[Otto Nobedder]

Jim IS a valuable source of information.

He's very careful that his information is valuable regardless of the machine you use for the process, and we should all appreciate that. It's a hard line to walk when you represent a particular maker, to share information without "advertising". Jim does so well at that, that he represents his company by default. Well played, and helpful to all.

Steve S