How to Make Patterns for a Plasma CNC Machine

• 1
  Key takeaways
• 2
  Why the pattern decides what a plasma CNC machine can hold
• 3
  Step 1: Define requirements before opening CAD
• 4
  Step 2: Draw geometry that survives CAM import
• 5
  Step 3: Apply kerf compensation and lead-ins
• 6
  Step 4: Nest the sheet and post the program
• 7
  Step by step: from drawing to first good part
• 8
  Kerf, web, and lead-in by plate thickness

A pattern for a plasma CNC machine is a 2D vector file plus the machine instructions that go with it. The drawing supplies geometry. The toolpath supplies order, direction, lead-ins, and speed. Skip the second half and the torch still fires, but the part will not match the print.

Three things travel with every pattern: material grade and thickness, kerf width for that thickness, and the pierce point rules for the machine. Change any one and the pattern has to be reissued. A DXF alone is not a pattern.

We keep patterns per thickness and per material. A 6 mm mild steel job cut at 130 A behaves nothing like the same outline in 12 mm plate at 200 A. Edge squareness drifts, dross forms, and hole diameters shrink by 0.3–0.8 mm depending on the cut.

That is the core trade: a pattern is a commitment to one set of cutting conditions. Engineers who treat it as a reusable template usually cut the first article twice.

Pattern work also decides how much of the sheet you throw away. A nest with 8 mm web spacing on 3 mm plate holds together well. The same spacing on 10 mm plate distorts as the heat builds up between cuts.

None of this needs a 5-axis machine. A clean 2D workflow removes most of the risk before the plate ever reaches the table.

Write down five numbers first: material grade, plate thickness, overall part size, hole size range, and the quantity you need from one sheet. These five drive every later choice, and they take ten minutes to settle.

Grade and thickness set the amperage range. 1–3 mm mild steel runs around 30–60 A. 6 mm sits near 100–130 A. 12 mm and up needs 170–200 A and a different consumable set. Stainless and aluminum shift those numbers again.

Hole size is the limit most people miss. Plasma cuts holes under about 1.5× the plate thickness with a tapered wall. A 10 mm hole in 12 mm plate will not hold a tight fit. If the print calls for that, plan to drill or ream after cutting.

Quantity decides nesting strategy and how much scrap you tolerate between parts. One-off jobs favor a loose nest. A 200-part run justifies the time to tune web spacing and common-line cuts.

Finally, note any cosmetic face. Plasma leaves a heat-affected zone and a rougher edge on the bottom side. If one face shows, the pattern should place that face up.

Get these five written down and the rest of the steps become mechanical.

Draw at 1:1 in millimeters or inches, never scaled. CAM software reads model units, and a drawing made at 1:2 will cut at half size. Check the import dialog before you accept it.

Keep every contour as a single closed polyline. Open contours force the operator to guess the start and end point, and plasma needs a clean pierce and a clean lead-out. Close everything.

Remove zero-length segments, duplicate lines, and stray points. These are the top cause of a machine that stops mid-cut or drops a pierce. Use the overkill or purge command in your CAD tool and then re-check the contour count.

Keep a minimum inside corner radius of about 1.5 mm. A sharp internal corner cannot be cut by a round torch; the arc simply cannot reach it. The corner will come out rounded or burned. Design the radius in.

Text and logos need a stroke width of at least 1.2 mm if they are cut as letters. Thinner strokes lose detail to the kerf. For anything finer, cut it as an outline and mark it instead.

We build patterns for client parts in Fusion 360 and Mastercam, then export DXF for the cutting table. The geometry rules above apply no matter which tool you use.

Kerf is the width of material the arc removes. For a plasma CNC machine it typically runs 0.8 mm at 30 A up to 2.5 mm at 200 A. The cut path sits half the kerf outside the finished edge for an external profile, and half inside for a hole.

Get the offset direction wrong and every part comes out 1.5–5 mm undersized. That is the single most common pattern error we see in incoming files. Check the offset side on one contour before you post the whole nest.

Lead-ins should be at least 1.5× the kerf long, and they must start on scrap, not on the part edge. A 6 mm lead-in on a 12 mm plate is too short; the pierce crater will eat into the finished edge.

Use a straight lead-in for mild steel and an arc lead-in when the part edge is cosmetic. Arc lead-ins leave a smoother entry and less notch. Both must clear the part outline by the full kerf width.

Add a lead-out on thick plate. Without one, the torch dwells at the end point and burns a divot. A 3–5 mm lead-out past the start point clears it.

Holes under 12 mm should be cut at reduced speed, roughly 60–70% of the profile speed. The slower travel keeps the arc stable through the small radius.

Finally, set the pierce height and cut height in the toolpath, not at the console. Pierce height is usually 1.5–3 mm above the plate; cut height is 1.0–1.5 mm.

Nest parts with a web of at least 6 mm on plate up to 6 mm thick, and 10–12 mm on plate over 10 mm. Thin webs warp under heat and the parts shift.

Group parts by material and thickness before nesting. Mixing 3 mm and 10 mm on one sheet forces a program change mid-run and wastes setup time.

Cut inside holes before the outer profile. If the outer profile goes first, the part can shift and the holes land off-center. Every CAM package supports this order; verify it in the simulation.

Choose the pierce point on scrap whenever possible. On a nested sheet, the gap between parts is scrap. Pierce there and the part edge stays clean.

Post the program and run a dry simulation at full speed. Watch for rapid moves that cross a finished contour. A rapid across a cut path can clip a part that already released.

Save the DXF, the CAM file, and the posted G-code together, with the material and thickness in the filename. Six months later nobody remembers which file ran on 6 mm versus 8 mm plate.