The core DFM rules for laser-cut sheet metal are simple and all scale with material thickness (t): a hole diameter should be ≥ the material thickness, a hole should sit ≥ 1.5× t (or ≥ its own diameter) from any edge, holes should be ≥ 2× t apart centre-to-centre, and any hole should clear a bend by ≥ 2× t plus the bend radius. Stay above these and the laser holds clean edges with flat, undistorted webs. Go below them and edges round over, thin webs melt or warp, and holes deform when a nearby bend is formed. This page states each rule answer-first, with the verified number and the physical reason behind it, so you can lay out features correctly before sending the file.
This is the feature-spacing companion to our broader design-for-manufacturing guide and sheet metal tolerances chart.
What are the minimum hole and edge rules for laser-cut sheet metal?
Every minimum below is expressed as a multiple of material thickness t, because that is what actually drives the physics — a rule that works on 1mm sheet has to scale up for 10mm plate. This is the master reference table; the sections that follow explain each line.
| Feature | Minimum rule | Why it exists |
|---|---|---|
| Hole / slot diameter | ≥ t (min 1mm) | Below 1× t the beam can’t fully form a clean round hole; the edge rounds over |
| Hole / feature to edge | ≥ 1.5× t, or ≥ 1× hole Ø (use the larger) | Thin rim between hole and edge overheats, melts or bows outward |
| Hole to hole spacing | ≥ 2× t centre-to-centre; ≥ 6× t preferred | Thin web between two holes distorts and loses flatness |
| Hole to bend | ≥ 2× t + bend radius (from hole edge to bend line) | Forming pulls and ovals any hole inside the bend deformation zone |
| Slot width | ≥ t wide; ends ≥ 1.5× t from edge | Narrow slots close up from kerf and heat |
| Web / bridge between cuts | ≥ t (1–1.5× t preferred) | Thin strips between two cuts melt or warp from heat |
| Inside bend radius | ≥ t | Tighter radii crack the outer fibre, worst on hard stainless / aluminium |
| Min flange height (leg of a bend) | ≥ 4× t | A shorter flange can’t be gripped by the press-brake die |
| Internal corner radius | ≥ 0.5mm | A laser beam has finite width; truly sharp internal corners are not cuttable |
The single rule to remember: when in doubt, keep features at least one full thickness away from anything — another hole, an edge, or a bend — and you’ll rarely hit a manufacturability problem.
How small a hole can a laser cut?
The smallest reliable laser-cut hole has a diameter equal to the material thickness — Ø ≥ t — with a practical floor of about 1mm. On 2mm sheet, the smallest clean hole is roughly Ø2mm; on 10mm plate it is roughly Ø10mm.
The limit comes from how the beam pierces and forms the hole. The laser has to enter the material, travel around a closed contour, and exit at the pierce point. When the diameter drops below one thickness, the beam doesn’t have room to complete a clean circle — the entry pierce overlaps the contour, the bottom edge rounds over, and the dross can’t clear. The hole comes out tapered, oval, or partly bridged.
If you need a smaller hole than 1× t — for example a Ø1.5mm hole in 4mm plate — that is a job for drilling or a secondary machining pass, not the laser. Call it out on the drawing and we plan it into the quote rather than failing it on the laser.
How far must a hole be from the edge?
Keep at least 1.5× material thickness — or one hole diameter, whichever is larger — between the edge of a hole and the edge of the part. On 3mm sheet that is a minimum 4.5mm rim; on a large hole, use the hole’s own diameter as the floor instead.
The rim of metal between a hole and the part edge is a thin, unsupported strip. The laser dumps heat into it from both sides at once — the cut around the hole and the cut along the edge — and a strip narrower than ~1.5× t can’t shed that heat fast enough. It overheats, bows outward, or melts through, leaving a ragged edge or a blown-out rim.
Thicker material needs a proportionally wider rim because it carries more heat per cut. This is also why edge-of-part holes on enclosure flanges should be moved inboard whenever the design allows — a fastener hole right at the lip of a panel is both a cutting risk and a weak point in service.
How far apart must holes be?
Holes should sit at least 2× material thickness apart, measured centre-to-centre, and ideally 6× thickness apart for a clean, flat result. On 2mm sheet that is a 4mm absolute minimum and ~12mm comfortable spacing; on 6mm plate, 12mm minimum and ~36mm comfortable.
The constraint is the web — the strip of solid metal left between two holes. A narrow web has metal being cut away on both sides, so it heats from both edges and has very little mass to stay flat. Below ~2× t the web can sag, bow, or distort, throwing off both hole positions. At ~6× t and above, the web behaves like normal sheet and stays flat, which is why dense bolt patterns and perforated panels are tolerance-checked against this number.
| Hole spacing (centre-to-centre) | Result |
|---|---|
| < 2× t | Web too thin — risk of distortion or melt-through; not recommended |
| 2× t (absolute minimum) | Cuttable, but inspect the web for warp |
| ≥ 6× t (preferred) | Web stays flat; positions hold to standard tolerance |
How close can a hole be to a bend?
Keep any hole at least 2× material thickness plus the inside bend radius away from the bend line, measured from the edge of the hole. A hole inside that zone gets pulled out of round when the bend is formed.
When a press brake forms a bend, the metal in the bend deformation zone stretches on the outside and compresses on the inside. Any hole that sits inside this zone is dragged along with the metal: a round hole becomes an oval, its position shifts, and on tight radii the rim can tear. Because the deformation zone widens with both thickness and bend radius, the safe clearance is the sum of the two — roughly 2× t + R from the hole edge to the bend line.
If a hole genuinely has to be close to a bend (common on small brackets), there are two reliable fixes: cut the hole after bending as a secondary operation, or add a small relief slot at each end of the bend so the deformation stops short of the hole. Both add cost, so design the clearance in from the start where you can.
Minimum flange and tab dimensions
A bent flange — the leg of metal standing up from a bend — should be at least 4× material thickness tall, and a tab should be at least 2× its own thickness wide. Below these, the press brake physically can’t form or grip the feature.
- Flange height ≥ 4× t. The press-brake die needs enough material on each side of the bend to clamp and form it. A flange shorter than ~4× t sits over the die opening with nothing to hold, so it bends inconsistently or not at all. On 2mm sheet that is an 8mm minimum flange; on 4mm, 16mm.
- Tab width ≥ 2× t (min ~4–5mm). A narrow tab cut from sheet has little mass and heats up fast at the laser; it also bends erratically. Keep tabs at least twice as wide as they are thick.
- Notch / cutout width ≥ t. Internal slots and notches follow the same web logic as holes — keep them at least one thickness wide so the surrounding metal stays flat.
- Hem / safety edge: a closed hem needs a flat length of roughly 4× t before the return; tighter and the press can’t tuck it.
| Bent feature | Minimum dimension |
|---|---|
| Flange height (leg of a bend) | ≥ 4× t |
| Tab width | ≥ 2× t (min ~4–5mm) |
| Inside bend radius | ≥ t |
| Slot / notch width | ≥ t |
| Distance from hole to bend (hole edge → bend line) | ≥ 2× t + R |
These forming rules pair with the cut-feature rules above; see our press brake bending essentials and the material thickness capability guide for the bending and thickness limits behind them.
Why these rules exist (heat, tool access, distortion)
Every rule on this page traces back to one of three physical causes — and naming them makes it easy to judge a feature the table doesn’t explicitly cover.
- Heat. A fiber laser cuts by melting and vaporizing metal, dumping a lot of energy into a small area. Any thin strip of metal — a narrow rim, a slim web, a tiny tab — can’t shed that heat fast enough and overheats, melts, or warps. This is why almost every minimum is “keep enough metal around the feature.”
- Beam and tool access. The beam has a finite diameter (it leaves a kerf of roughly 0.08–0.45mm), so it can’t form a perfectly sharp internal corner or a hole smaller than it can cleanly pierce. The press-brake die needs room to grip a flange. Geometry the tool can’t physically reach can’t be made on that machine.
- Forming distortion. Bending stretches and compresses metal in a zone around the bend. Holes, slots, and edges inside that zone get dragged out of shape. The “clear the bend by 2× t + R” rule is purely about staying outside the distortion zone.
When you meet a feature these rules don’t cover, ask which of the three is at play: Is there enough metal around it to absorb heat? Can the tool physically reach it? Is it clear of any forming? If all three are yes, it’s almost always manufacturable.
What happens if you violate a rule?
You don’t always get a hard reject — more often you get a part that’s subtly wrong and costs money to discover. Typical outcomes:
| Rule violated | Likely result |
|---|---|
| Hole Ø < t | Rounded-over, tapered or oval hole; may not pierce cleanly |
| Hole too close to edge | Melted, bowed or blown-out rim; weak edge in service |
| Holes too close together | Distorted web; both hole positions drift out of tolerance |
| Hole too close to a bend | Hole ovals and shifts when formed; rim may tear |
| Flange < 4× t | Bend forms inconsistently or the press can’t grip it |
In practice we DFM-check every incoming DXF and flag features that break these rules before cutting, then suggest the smallest change — nudge a hole inboard, add a relief slot, split a feature into a secondary operation — so the first article passes. We can also supply Mill Test Certificates (MTC) and first-article inspection on request; ISO 9001 is in progress.
FAQ
What is the minimum distance from a hole to the edge of sheet metal? At least 1.5× the material thickness, or one hole diameter, whichever is larger. On 3mm sheet that’s a minimum 4.5mm rim. A thinner rim overheats and bows outward at the laser.
What is the minimum hole spacing for sheet metal? At least 2× material thickness centre-to-centre as an absolute minimum, and 6× thickness for a flat, distortion-free web. Dense bolt patterns and perforated panels should target the 6× figure.
How close can a hole be to a bend? Keep the hole edge at least 2× thickness plus the inside bend radius from the bend line. Inside that zone the forming action ovals the hole. If it must be closer, cut the hole after bending or add a relief slot.
Can you cut countersunk or threaded holes? A laser cuts the pilot hole; countersinks and tapped threads are secondary operations (machining, or PEM-style press-in hardware). Call them out on the drawing and we plan them into the job in-house.
What is the minimum slot width a laser can cut? About one material thickness. Below that, kerf and heat close the slot up or melt the surrounding web. Keep slot ends at least 1.5× thickness from any edge.
What happens if my design breaks one of these rules? We flag it on DXF review before cutting and propose the smallest fix — moving a feature, adding a relief, or a secondary operation — rather than producing a bad first article.
Get your part DFM-checked
Send your DXF and we’ll review every hole, edge and bend against these rules, then tell you exactly what (if anything) to change before we cut — on our 6kW fiber laser in Bình Dương, Vietnam. Request a free DFM review and quote — or read the full design-for-manufacturing guide first.
