Tips for a Miller CNC Plasma Table
A Miller CNC plasma table cuts well when the consumables, torch height and cut chart all agree. This guide walks through seven checks we run on plasma-cut steel before a part goes to the mill. Written for operators and shop engineers who need square edges and repeatable holes, not just a cut line.
In this article
- 1
- 2
- 3
- 4
- 5
- 6
- 7
- 8
- 9
What matters most on a Miller table
How a Miller CNC plasma table actually cuts
A Miller CNC plasma table pairs a plasma power supply with an X-Y gantry and a height controller. The power supply strikes an arc between a tungsten electrode and a copper nozzle, then forces compressed air or nitrogen through that arc. The gas becomes a plasma jet at roughly 20,000–30,000 °C, which melts the steel and blows the molten metal out the bottom of the kerf.
Because the process is thermal, the cut edge is not a machined edge. Expect a slight bevel, a heat-affected zone and a rougher surface than milling. On 6 mm mild steel a well-tuned table gives roughly a 2–5° bevel on the right-hand side of the cut and a surface around Ra 12–25 μm. That is normal, not a defect.
Miller tables are usually paired with integrated controllers and Hypertherm-style torches, and the cut charts in the manual are the reference point for amperage, feed rate and gas pressure. The tips below assume you follow those charts first, then adjust for your material batch. If the chart number and the cut result disagree, the machine is usually right and the material is the variable.
One thing worth stating up front: plasma cuts 2D profiles. It does not produce bores, threads, counterbores or tight tolerances. When a drawing calls for ±0.05 mm on a hole pattern, the plasma table makes the blank and a CNC mill finishes it. Mixing those two steps is where most shops save money.
Inspect electrodes, nozzles and shields before every job
The electrode and nozzle are the two parts that define the arc. The electrode has a hafnium or tungsten insert that erodes with every start. The nozzle has a bore that widens as it wears. Once that bore grows, the arc spreads, the kerf gets wider and the cut edge turns rough and drossy. No control setting fixes a worn nozzle.
Pull the consumables and look at them under good light. A healthy electrode insert is a shallow, even crater. A deep pit, a greenish tint or a white powdery ring means the electrode is done. A healthy nozzle bore is round with a sharp edge. An oval bore, a nick, or a bright ring around the orifice means replace it.
Track pierces per set. On a typical 45–65 A setup cutting 6 mm mild steel, expect roughly 800–1,200 pierces from an electrode and about half that from a nozzle. Log the count on the machine and change both at the same time. Changing only the nozzle leaves a worn electrode dumping heat into the new part.
Check the shield cup and swirl ring too. A cracked shield changes the gas flow and causes an arc that wanders. A swollen or dirty swirl ring does the same. Both are cheap. Replace them whenever you change the electrode and nozzle, and keep a sealed spares box next to the table.
- 1ElectrodeShallow even crater is fine; deep pit or green tint means replace.
- 2NozzleBore must be round and sharp. Oval or nicked bore ruins the kerf.
- 3Shield and swirl ringAny crack, swelling or oil film disturbs gas flow. Replace with the set.
- 4Log piercesAbout 800–1,200 pierces per electrode at 45–65 A on 6 mm steel.
Set pierce height and cut height separately
Torch height control is the single biggest lever on cut quality after consumables. Two heights matter: the pierce height, where the arc starts, and the cut height, where the torch rides during the cut. They are not the same number and they are not interchangeable.
Pierce at 1.5–2× the cut height, so around 2.5–4.0 mm above the plate on a 45–65 A setup. Piercing too close blows molten metal back into the nozzle and shortens its life. Pierce too far and the arc does not transfer cleanly, leaving a ragged start point.
Once the arc transfers and the pierce delay elapses, the THC drops the torch to the cut height from the chart, typically 1.0–1.5 mm. That gap controls the kerf width and the bevel. Rise above 2 mm and the cut edge starts to taper badly. Drop below 0.8 mm and you risk a collision with a tipped-up part.
Set the pierce delay from the chart, usually 0.3–0.8 s on 6 mm steel, and lengthen it on thicker plate. If the torch moves before the arc fully penetrates, the start of every cut will have a notch. If the delay is too long, you get a blown-out pierce hole. Test on a scrap plate and measure the pierce dimple before running production.
Voltage-based THC needs a calibration pass. Run a test cut on scrap, watch the arc voltage on the controller, and confirm the height reading matches a physical measurement with a feeler gauge. If the two disagree by more than about 0.3 mm, recalibrate before you cut parts.
Clean, dry air is not optional
Plasma air carries the arc energy and blows the molten metal out. If that air contains water or oil, the arc becomes unstable and the cut edge shows porosity, black smears and heavy dross. Operators often blame the torch when the real problem is a saturated dryer.
Filter the air at three points: at the compressor outlet, at the main line, and at the machine inlet. A refrigerated dryer plus a coalescing filter gets most shops to a usable point. Check the filter elements monthly and drain the separator bowl daily. A bowl half full of water will pass moisture straight to the torch.
Pressure at the machine inlet should sit where the cut chart says, commonly 5.5–6.9 bar (80–100 psi) for a 45–65 A setup. Pressure that sags during a cut means the supply line is undersized or the filter is clogged. Watch the gauge during a long cut, not at idle.
Nitrogen gives a cleaner edge on stainless and aluminum than shop air, but it costs more per part. Use it where the cut edge is visible or where the part gets welded without cleanup. For plain mild steel blanks headed to the mill, filtered shop air is enough.
Read the dross to find the real problem
Dross is the resolidified metal that sticks to the bottom or top edge of a cut. Its location tells you what to change. Slow dross is a heavy, bubbly bead on the top edge, and it means the feed rate is too low or the torch is too high. The arc stays in one spot too long and the puddle grows.
Fast dross is a thin, hard, tightly bonded line on the bottom edge with a slight lag in the cut. That means the feed rate is too high or the amperage is too low. The arc leans back and does not fully clear the kerf. Reduce speed in 10% steps and recheck before you touch the amperage.
Edge rounding on the top corner points to excessive cut height or a worn nozzle. A taper that gets worse along the cut usually means the torch is not perpendicular to the plate, or the plate is warped and the THC is chasing it. Check square with a machinist square on a fresh coupon.
For mild steel under 12 mm, a light grind removes most dross. For stainless and aluminum, dross is tougher and often needs a flap disc or a tumbling pass. If the part will be machined anyway, leave 1.5–2.5 mm of stock on the plasma edge and let the mill clean it up. That is faster than fighting the dross.
Plan the cut sequence to control heat
Heat is the enemy of flat plate. A long cut running down one side of a sheet heats that strip and it bows. The next cut then runs at a different height and the part comes out tapered. Sequencing is how you avoid this without slowing the machine.
Cut small holes and internal features first, then the outer profile last. If you cut the outer profile first, the part can shift or tip and the torch will crash into it on the next feature. Leave tabs or a micro-joint of 0.5–1.0 mm so the part stays attached until the end.
Spread the heat. Alternate between opposite ends of the sheet rather than working left to right in one pass. On thin sheet under 3 mm, expect warp regardless and plan for it: nest parts with a common-line cut or add a skim pass. On 10 mm and above, heat is less of a problem and you can nest tightly.
Lead-ins matter too. Start the pierce in the scrap area, not on the part edge, and run the lead-in at least the material thickness long, commonly 5–10 mm. A pierce on the part edge leaves a notch that shows up on the finished part. For holes, a curved lead-in gives a cleaner entry than a straight one.
Seven-step setup routine before a production run
Run these in order. Skipping a step moves the error to the next one instead of removing it.
- 11. Inspect and log consumablesPull the electrode, nozzle, shield and swirl ring. Check the electrode crater and the nozzle bore under light. Record the pierce count. Replace all four as a set if any one is worn.
- 22. Check air supply and filtersDrain the separator bowl. Confirm inlet pressure at 5.5–6.9 bar during a cut, not at idle. Replace the coalescing filter element if it looks discolored or has been in service over a month.
- 33. Verify plate flatness and groundingLay the plate on the slats and check for rock. Clamp the work lead directly to the plate, not to the table frame, and clean the contact point. Poor ground causes arc wandering.
- 44. Set pierce height and cut heightPierce at 2.5–4.0 mm, cut at 1.0–1.5 mm for a 45–65 A setup. Confirm with a feeler gauge on a test move. Do not trust the screen number alone.
- 55. Load the cut chart and test on scrapEnter the amperage, feed rate, pierce delay and gas pressure from the chart. Cut a 200 mm coupon and check the kerf width, bevel and dross before running parts.
- 66. Run the nest with heat-aware sequencingHoles and internal features first, outer profile last with a 0.5–1.0 mm tab. Alternate cuts across the sheet. Watch the arc voltage during the first part.
- 77. Inspect the first part fullyMeasure the profile, check square, check hole size. If the first part is good, the run is good. If it is off, stop and find the cause before cutting the rest of the sheet.
Plasma or mill: which process for which feature
Use this when a drawing mixes cut profiles with machined features.
| Feature | Plasma table | CNC milling | Rule of thumb |
|---|---|---|---|
| Outer profile, 3–25 mm plate | Fast, ±0.25 mm typical | Slower, ±0.005 mm | Plasma for the blank |
| Holes under 1.5× thickness | Oversized, tapered | Round and on size | Mill the holes |
| Hole tolerance ±0.05 mm | Not achievable | Standard | Mill after plasma |
| Bevel on edge | 2–5° typical | Square within 0.05 mm | Mill if square matters |
| Surface finish | Ra 12–25 μm | Ra 0.8–1.6 μm | Mill for sealing faces |
| Threads and counterbores | Not possible | Standard | Mill only |
| Flatness on thin sheet | Warps without care | Stable if clamped | Plasma plus stress relief |
| Cost per part at volume | Low setup, low cycle | Higher cycle, tight result | Plasma blank, mill finish |
When the plasma table is the wrong tool
If the drawing calls for holes under 1.5× material thickness, a square edge or a sealing face, the plasma table makes the blank and a CNC mill finishes it. We take plasma-cut plate and machine it to ±0.005 mm across 127 CNC machines, with 5-axis capacity up to 4,000 mm and no minimum order quantity.
Miller CNC plasma table questions
How often should I change consumables on a Miller CNC plasma table?
Track pierces rather than hours. At 45–65 A on 6 mm mild steel, an electrode typically lasts about 800–1,200 pierces and a nozzle about half that.
Replace electrode, nozzle, shield and swirl ring as a set. Changing one worn part while leaving the others just moves the damage to the new part.
Why does my plasma cut have dross on the bottom edge?
Bottom dross with a lag in the cut usually means the feed rate is too high or the amperage is too low. Reduce speed in 10% steps and recheck before changing amperage.
Check air quality as well. Moisture or oil in the line produces the same symptom and no speed change will fix it.
What tolerance can a Miller CNC plasma table hold on holes?
On holes smaller than about 1.5× the material thickness, expect roughly ±0.25 mm at best, often worse, and the hole will taper. The arc cannot stay round as the kerf wraps a small diameter.
If the drawing needs ±0.05 mm, cut the hole undersize on the plasma table and bore it on a mill.
Can I plasma cut stainless and aluminum on the same machine?
Yes, but the settings change. Stainless and aluminum cut cleaner with nitrogen than with shop air, and they need different feed rates and pierce delays from mild steel.
Dross on stainless and aluminum is harder to remove. If the edge will be visible, factor in a grinding or tumbling pass.
Should I send plasma-cut plate to a machine shop?
If the part has tight holes, threads, counterbores or a sealing face, yes. Plasma makes the profile and the mill finishes the features. Leaving 1.5–2.5 mm of stock on the plasma edge gives the mill something to clean up.
If the part is a flat bracket with no critical features, the plasma cut is the finished part.
How do I stop thin sheet from warping on the table?
Sequence cuts so heat spreads across the sheet instead of concentrating in one area, and cut holes before outer profiles.
On sheet under 3 mm, some warp is normal. Nest with common-line cuts or plan a skim pass, and clamp the plate if flatness matters.
Plasma blank, milled to tolerance
Send us your plasma-cut plate or a 2D drawing. We quote within 12 hours with a free DFM analysis, and parts ship in 3–5 days.
12-hour quote±0.005 mm100% inspectionNo minimum order
More from the shop floor
We publish setup notes, tooling trials and inspection data from the factory floor.
