Sheet Metal Hole Size & Minimum Feature Quick Chart

Q: What is the minimum laser-cut hole size in sheet metal?

Use a hole diameter at least equal to material thickness (D >= T) as a conservative cross-supplier starting point. A validated fiber-laser system may cut below T, but the acceptable limit depends on material, thickness, gas, piercing strategy, taper, dross, roundness, and the supplier’s parameter set.

Q: How close can a hole be to a sheet-metal edge?

For punching, begin with a clear ligament of at least 2T from the hole edge to the free sheet edge. Convert that to a centerline dimension by adding half the hole diameter: C_e >= D/2 + 2T.

Q: How far should a hole or slot be from a bend?

As an early DFM convention, measure at least R + 2.5T from the nearest round-hole edge to the bend tangent line and R + 4T from the nearest slot edge. Because supplier guides do not always use the same bend-line reference, show the measurement origin explicitly and confirm both values against the real material, radius, V-die, bend angle, direction, sequence, and tooling.

Q: What is the minimum slot width in sheet metal?

Use a slot width at least equal to material thickness (S >= T) as a general DFM starting point. A narrower laser-cut slot may be possible on a validated system, but pierce placement, dross, taper, heat, and narrow-web distortion need review.

Sheet Metal Hole Size & Minimum Feature Quick Chart

Use actual material thickness—not a nominal gauge number—as T. Where a distance is described as clear, measure from the nearest cut edge of one feature to the nearest edge of the next feature, not from centerline to centerline.

Feature or check	Early DFM starting point	Measurement basis	Practical note
Laser-cut round hole	D >= T	Finished nominal diameter	Conservative cross-supplier rule; a validated fiber-laser process may go below T
Laser-cut slot	S >= T	Minimum clear slot width	Narrow slots are sensitive to pierce size, heat input, lead-in location, dross, and distortion
Punched hole, aluminum, non-guided tool	D >= 0.75T	Punch diameter or narrowest tool width	Mate published ratio; confirm tool availability, guidance, stripping, and maintenance
Punched hole, mild steel, non-guided tool	D >= 1.0T	Punch diameter or narrowest tool width	Good general punching screen for maintained standard tooling
Punched hole, stainless steel, non-guided tool	D >= 2.0T	Punch diameter or narrowest tool width	Higher load and punch-breakage risk require a larger ratio
Punched hole, aluminum, fully guided tool	Published guidance can reach D >= 0.5T	Tool-specific	Requires a compatible fully guided tooling family and process review
Punched hole, mild steel, fully guided tool	Published guidance can reach D >= 0.75T	Tool-specific	Do not assume the ratio applies to ordinary non-guided tooling
Punched hole, stainless steel, fully guided tool	Published guidance can reach D >= 1.0T	Tool-specific	Confirm material strength, die clearance, press alignment, and tool life
Punched hole to free edge	Clear ligament E >= 2T	Hole edge to sheet edge	Reduces edge bulging, breakout, tearing, and distortion
Between punched holes	Clear web W >= 2T	Hole edge to hole edge	Protects the narrow web and reduces interaction between hits
Round hole to bend	H >= R + 2.5T	Hole edge to bend tangent line	This chart uses an edge-to-tangent convention; confirm the supplier's bend-line convention
Slot to bend	B_s >= R + 4T	Slot edge to bend tangent line	This chart uses an edge-to-tangent convention; slots interact with a larger deformation zone
Notch width	One general DFM starting point: N >= 1.5T	Narrowest clear notch width	Supplier guides vary; confirm the cutting process, deburring method, and feature function
Notch length	Width-based slenderness check: L_n <= 5N	Length relative to notch width	Some guides use thickness-based limits instead; state and confirm the selected convention
Tab width	B_t >= max(2T, 3.2 mm)	Narrowest tab width	General DFM reference; confirm if the tab is structural, welded, or repeatedly handled
Tab length	L_t <= 5B_t	Length relative to tab width	Long slender tabs can twist, bow, or overheat
Inside notch corner radius	Start at r >= 0.5T	Internal cut radius	A radius reduces stress concentration and avoids an artificially sharp laser corner
Self-clinching hardware hole	Use the exact manufacturer series value	Finished mounting-hole diameter and tolerance	Thread size alone does not define the correct clinching hole
Drilled or reamed precision hole	No universal D:T ratio	Finished diameter, tolerance, position, and surface requirement	Use machining when fit, true position, cylindricity, or surface quality controls the design

Where:

T = actual material thickness
D = nominal round-hole diameter
S = minimum slot width
E = clear ligament from a hole edge to a free sheet edge
W = clear web between adjacent hole edges
R = specified inside bend radius
H = clear distance from a round-hole edge to the bend tangent line
B_s = clear distance from a slot edge to the bend tangent line
N = notch width
B_t = tab width

These dimensions solve different problems. The hole-size ratio protects the cutting or punching process; the edge and web rules preserve surrounding material, the bend-distance rules keep features outside the forming deformation zone.

How to Use This Minimum Feature Chart

Apply the chart in the following order:

Specify the material grade or alloy, temper or condition, and actual thickness.
Identify whether the feature will be laser cut, punched, drilled, reamed, or selected by the fabricator.
Calculate the minimum hole or slot dimension for that process.
Round upward to an available punch, drill, reamer, or practical programmed diameter.
Check the clear material around the feature: edge ligament, hole-to-hole web, and nearby notches or slots.
Check the distance from the feature edge to the bend tangent line using the intended inside radius.
Decide whether the feature is a clearance opening or a functional precision bore.
Define diameter, tolerance, position, datums, burr direction, finish condition, and inspection method where function requires them.

A minimum-size feature can pass one check and still fail another. For example, a 2.0 mm laser-cut hole in 2.0 mm sheet satisfies D >= T, but it may still distort if placed inside the bend zone or break out if too close to an edge.

Converting clear distances to drawing dimensions

If a drawing dimensions a hole from its center, convert the clear-ligament rules explicitly.

For a hole center to a free edge:

C_e >= (D / 2) + 2T

For the center-to-center pitch between two holes:

P >= (D_1 / 2) + (D_2 / 2) + 2T

For a round-hole center to the bend tangent line:

C_b >= (D / 2) + R + 2.5T

Where C_e is center-to-edge distance, P is hole pitch, and C_b is hole-center-to-bend-tangent distance.

For two equal 4.0 mm holes in 2.0 mm sheet, the early punched-feature checks give:

Center to free edge: C_e >= 2.0 + 4.0 = 6.0 mm (0.236 in)
Hole center-to-center pitch: P >= 2.0 + 2.0 + 4.0 = 8.0 mm (0.315 in)
With an inside bend radius of 2.0 mm, center to bend tangent: C_b >= 2.0 + 2.0 + 5.0 = 9.0 mm (0.354 in)

State the measurement origin on the drawing. A note such as “6 mm from edge” is ambiguous unless it is clear whether the dimension controls the hole center or the remaining ligament.

Minimum Punched Hole Size by Material and Thickness

The table below calculates non-guided punch starting diameters from Mate’s published ratios. Aluminum values are rounded upward to the next 0.1 mm. Metric values control; inch equivalents are rounded to the nearest 0.001 in for reference and should not be used to infer a tighter manufacturing tolerance. These are calculations, not a catalog of available punch sizes and not a guarantee that a particular press can use the resulting tool.

Sheet thickness T	Aluminum at 0.75T	Mild steel at 1.0T	Stainless steel at 2.0T
0.8 mm (0.031 in)	0.6 mm (0.024 in)	0.8 mm (0.031 in)	1.6 mm (0.063 in)
1.0 mm (0.039 in)	0.8 mm (0.031 in)	1.0 mm (0.039 in)	2.0 mm (0.079 in)
1.2 mm (0.047 in)	0.9 mm (0.035 in)	1.2 mm (0.047 in)	2.4 mm (0.094 in)
1.5 mm (0.059 in)	1.2 mm (0.047 in)	1.5 mm (0.059 in)	3.0 mm (0.118 in)
2.0 mm (0.079 in)	1.5 mm (0.059 in)	2.0 mm (0.079 in)	4.0 mm (0.157 in)
3.0 mm (0.118 in)	2.3 mm (0.091 in)	3.0 mm (0.118 in)	6.0 mm (0.236 in)
4.0 mm (0.157 in)	3.0 mm (0.118 in)	4.0 mm (0.157 in)	8.0 mm (0.315 in)
6.0 mm (0.236 in)	4.5 mm (0.177 in)	6.0 mm (0.236 in)	12.0 mm (0.472 in)

The ratios describe punch strength and tooling risk, not finished-hole quality. A punched wall normally includes rollover, burnish, fracture, and an exit burr. If the hole receives a dowel, bearing, precision pin, or close-fit fastener, punching may create a pilot that is machined to final size.

Use sheet metal punching when repeat volume, standard tool sizes, and fast cycle time support the tooling approach. Request a tooling review when the diameter approaches the ratio limit, the material has high shear strength, the web is narrow, or cosmetic/burr requirements are strict.

Minimum Laser-Cut Hole and Slot Size

For a broadly portable design, use a laser-cut hole diameter and slot width at least equal to material thickness:

Round hole: D >= T
Slot width: S >= T

The rule provides a practical starting point without assuming a specific laser source, power, nozzle, assist gas, focus position, piercing strategy, or proprietary small-contour cycle. It also leaves room for a supplier to change machines without invalidating every small feature in the drawing.

The rule is deliberately conservative. The Fabricator describes D >= T as the generally accepted laser-hole guideline, while also reporting that controlled fiber-laser processes can cut holes down to roughly one-quarter of material thickness in some conditions. That aggressive result is equipment- and quality-specific, not a universal replacement for D >= T.

Laser cutting services are useful for mixed hole sizes, irregular slots, prototypes, and low-to-medium volumes where dedicated punch tooling is not justified. When a hole or web is below T, request a supplier-specific review and define what “acceptable” means: entrance diameter, exit diameter, taper, roundness, dross, burr, recast, discoloration, and repeatability.

Why supplier laser charts can be smaller than T

247TailorSteel publishes system-specific minimum-hole values below material thickness. Selected values from its minimum-hole tables—using the nitrogen column for steel—include:

Sheet thickness	Steel minimum hole	Stainless minimum hole	Aluminum minimum hole
1.0 mm	0.5 mm	0.5 mm	0.5 mm
2.0 mm	1.0 mm	1.0 mm	1.5 mm
4.0 mm	2.0 mm	2.0 mm	2.5 mm
6.0 mm	4.0 mm	3.0 mm	4.0 mm

These values demonstrate what one validated production system accepts; they do not define ShincoFab capability or a general industry limit. Gas selection can also change the value—for example, the same supplier publishes different steel limits for nitrogen and oxygen at some thicknesses.

As holes and slots become smaller, the pierce occupies a larger share of the contour and heat has less room to dissipate. Common effects include:

entrance spatter or a pierce witness;
top-to-bottom diameter taper;
lead-in flatness or reduced roundness;
dross and directional burr;
local discoloration or recast;
melted or distorted narrow webs;
greater sensitivity to nesting, sheet flatness, and parameter changes.

If a small feature controls fit or alignment, the laser can create an undersized pilot while drilling, boring, or reaming establishes the final bore.

Hole, Slot, Edge, and Bend Clearance Rules

The material surrounding a hole often controls manufacturability more than the diameter itself.

Hole to free edge

Mate recommends at least 2T between a punched hole and the sheet edge. Treat this as the remaining clear ligament. For a minimum-diameter mild-steel hole where D = T, that converts to a center-to-edge dimension of 2.5T, which is why diagrams may show a larger centerline dimension than the written clear-distance rule.

A laser may physically cut a narrower ligament, but the remaining strip can discolor, warp, melt back, vibrate, or be damaged during deburring and handling. If a narrow bridge is required, state its minimum finished width and whether bow, discoloration, or edge rounding is acceptable.

Between holes

For punched features, begin with 2T of clear material between hole edges. Convert it to center-to-center pitch using the actual diameters. Avoid applying an undefined statement such as “holes must be 6T apart” without saying whether the dimension is clear web, center pitch, or edge distance.

Large hole patterns may also need review for sheet stiffness, distortion, press sequence, heat accumulation, and the percentage of open area. A web that survives one pair of holes may distort across a dense perforation field.

Hole to bend

For this chart, interpret the common R + 2.5T round-hole guideline and R + 4T slot guideline as clear distances from the nearest feature edge to the bend tangent line. Supplier guides do not always use the same bend-line reference, so show the measurement origin explicitly and confirm it against the fabricator’s flat-pattern and tooling method before releasing the drawing.

These are starting rules for conventional sheet-metal forming. The final requirement changes with bend angle, V-die opening, grain direction, relief geometry, material strength, and whether the hole is cut before or machined after bending. Establish a reasonable inside bend radius for the selected material and tooling before calculating the clearance.

When a critical hole cannot move outside the bend zone, consider drilling or reaming after forming, using a relief, changing the bend sequence, increasing the radius, or changing the part architecture.

Minimum Slots, Notches, Tabs, and Narrow Features

Round holes are not the only features that become fragile as their width approaches material thickness.

Feature	Early DFM reference	Main Failure Mode
Laser-cut slot width	S >= T	Pierce consumes the slot, walls taper, or slot closes with dross
Notch width	One general guide recommends N >= 1.5T	Narrow notch distorts, overheats, or becomes difficult to deburr
Notch length	Use L_n <= 5N as a width-based slenderness check	Long narrow notch twists or produces a weak tongue
Tab width	B_t >= max(2T, 3.2 mm)	Tab bends, bows, overheats, or breaks during handling
Tab length	L_t <= 5B_t	Slender tab loses positional stability
Inside notch radius	r >= 0.5T	Sharp internal corner concentrates stress and cannot remain perfectly sharp after laser cutting

These ratios are general DFM references rather than controlling standards. Published supplier guides use more than one notch-sizing convention; this chart adopts 1.5T for notch width and five times the notch width for length only as an early screening method. Confirm the final convention with the fabricator, and increase the dimensions for high-strength material, heavy deburring, structural tabs, welded attachments, cosmetic surfaces, or features exposed to repeated loading.

Do not confuse a slot width with its end radius or overall length. Dimension the clear width, end geometry, and location separately where the slot controls adjustment, airflow, a fastener path, or assembly access.

Hardware, Threads, Countersinks, and Precision Holes

Some features should not be designed from a generic thickness ratio.

Self-clinching hardware

A self-clinching fastener is selected by manufacturer, product family, thread, panel material, hardness, and thickness. A nut and a stud with the same thread can require different mounting holes. Use the exact diameter and tolerance from the chosen series rather than scaling the thread size. ShincoFab’s self-clinching fastener hole size chart provides examples and explains panel-thickness and edge-distance requirements.

Tapped holes

Specify the thread standard, class, pitch, pilot diameter, minimum engagement, panel condition, and whether the thread is cut, formed, extruded, or installed as hardware. Thin sheet may not provide adequate direct thread engagement even when the pilot hole can be cut.

Countersinks

Check screw standard, head angle and diameter, remaining material at the bottom of the countersink, distortion risk, and whether machining is required. A countersink that consumes most of the sheet thickness can create a sharp edge, breakout, or weak bearing surface. Do not infer a universal countersink depth from the minimum laser-hole rule.

Dowel, bearing, and locating holes

Laser cutting and punching can create useful pilots, but they do not automatically provide the cylindrical wall, close size, surface finish, and true position required for a precision fit. Drill, bore, interpolate, or ream when the functional tolerance demands it. A reamer improves an existing bore but normally follows the pilot; it should not be expected to correct a badly located hole.

For critical dimensions, compare the requirement with ShincoFab’s sheet metal tolerance chart and add explicit diameter, position, datum, inspection, and finish-condition callouts.

Design Checks Before Releasing a Drawing

Item	What to specify or confirm	Why it matters
Material	Grade/alloy, temper or condition, and applicable standard	Strength and ductility affect punching load, burr, forming, and crack risk
Thickness	Actual millimeter or decimal-inch thickness	Every ratio in the chart depends on T; gauge alone is material-specific
Process intent	Laser, punch, drill, ream, or supplier-selected	Prevents a precision requirement from being assigned to an unsuitable primary process
Feature function	Clearance, ventilation, locating, bearing, thread pilot, or cosmetic	Functional features need different tolerance and inspection controls
Diameter or width	Nominal value plus unilateral/bilateral tolerance where needed	Separates CAD geometry from acceptance criteria
Position	Datums and true position for mating patterns	Hole-size capability does not define location capability
Edge and web spacing	Clear distance and measurement convention	Prevents breakout, distortion, and ambiguous centerline interpretation
Bend relationship	Hole/slot edge, tangent line, inside radius, angle, and bend sequence	Prevents ovalization and feature movement during forming
Burr direction	Functional or cosmetic face	Punching, drilling, and cutting can leave directional burrs
Finish condition	Before or after deburring, forming, plating, anodizing, or powder coating	Secondary operations can change size, fit, and inspection results
Inspection method	Pin gauge, optical measurement, bore gauge, or CMM as appropriate	The method must reflect the functional requirement and tolerance
Quantity	Prototype, batch, or repeat production	Determines whether dedicated punching or secondary machining is economical

If the design started from gauge, convert it using the material-specific sheet metal gauge thickness chart before applying the ratios.

Common Minimum-Feature Problems

Symptom	Likely cause	Design or process response
Laser hole is tapered or not round	Hole is too small for the validated pierce/cut cycle	Increase diameter, approve a machine-specific limit, or machine the final bore
Narrow slot closes or fills with dross	Slot width and lead-in are too small	Increase width, move the pierce, change parameters, or machine the slot
Punch breaks or deflects	Punch-to-thickness ratio is too aggressive	Increase the feature, use fully guided tooling, or change process
High burr or galling	Tool wear, clearance, lubrication, or material adhesion	Review die clearance, tool condition, coating, and burr direction
Hole breaks out at the edge	Clear ligament is too small	Move the hole, enlarge the surrounding flange, or change the attachment method
Web between holes deforms	Adjacent features interact or the pattern removes too much material	Increase clear web, stagger hits, or review perforation sequence
Hole becomes oval after bending	Feature lies inside the bend deformation zone	Move the feature, add relief, or machine it after forming
Fastener will not fit after finishing	Coating, burr, taper, or inspection condition was not defined	Add masking/allowance, deburr, or machine after finish where required
Self-clinching hardware spins or pushes out	Wrong hole family, diameter, tolerance, panel hardness, or edge distance	Use manufacturer data and review installation sequence/tool access
Precision pin binds despite nominal diameter	Size alone was controlled; position, cylindricity, taper, or burr was not	Add GD&T and use an appropriate secondary machining/inspection process

What to Do When a Feature Is Below the Recommended Minimum

Option	When it helps	Trade-off
Increase the hole, slot, web, tab, or notch	Function permits more material or a larger opening	May affect fit, airflow, shielding, sealing, or appearance
Use a supplier-approved fiber-laser limit	Small-batch geometry can be validated on a specific laser	Reduces sourcing flexibility and may need first-article approval
Use fully guided punch tooling	Repeat volume justifies dedicated small-feature tooling	Adds tool cost, maintenance, and press-compatibility constraints
Cut an undersized pilot, then drill	A clean wall or smaller diameter is needed	Adds workholding, cycle time, and burr control
Ream or bore the final hole	Close fit, finish, or cylindrical geometry is critical	Requires machining access and does not automatically correct a poor pilot location
Machine the hole after bending	Forming would distort a critical feature	Adds a formed-part fixture and may restrict tool access
Move the feature or add relief	Edge or bend clearance is the limiting condition	Changes local geometry and may affect assembly space
Replace direct thread with inserted hardware	Sheet is too thin for adequate engagement	Requires a manufacturer-specific mounting hole and installation clearance
Split the geometry into separate parts	A tab, slot, or formed feature cannot be produced reliably	Adds joining, tolerance stack, labor, and possible distortion

Frequently Asked Questions

This FAQ gives conservative DFM starting points for sheet metal minimum features like holes, slots, edge clearances, and bend distances using actual thickness T. Use it for early design checks and confirm final manufacturability with your fabricator.

What is the minimum laser-cut hole size in sheet metal?

Use a hole diameter at least equal to material thickness (D >= T) as a conservative cross-supplier starting point. A validated fiber-laser system may cut below T, but the acceptable limit depends on material, thickness, gas, piercing strategy, taper, dross, roundness, and the supplier’s parameter set.

Can a laser cut a hole smaller than the sheet thickness?

Yes. Published supplier charts and fiber-laser case studies show below-thickness holes. Treat those values as machine-specific capability, not as a universal DFM rule or a ShincoFab guarantee. Request a sample when the hole is critical.

What is the minimum punched hole size in sheet metal?

For non-guided tooling, Mate publishes starting punch-to-thickness ratios of 0.75T for aluminum, 1.0T for mild steel, and 2.0T for stainless steel. Fully guided tooling can use smaller ratios, but only when the selected tooling family and press setup support them.

Why does stainless steel need a larger punched hole?

Stainless commonly imposes greater load and tool stress than aluminum or mild steel at the same thickness. A very narrow punch is more vulnerable to deflection, breakage, stripping loads, galling, and rapid wear, so ordinary non-guided tooling uses a more conservative ratio.

How close can a hole be to a sheet-metal edge?

For punching, begin with a clear ligament of at least 2T from the hole edge to the free sheet edge. Convert that to a centerline dimension by adding half the hole diameter: C_e >= D/2 + 2T.

How far should a hole or slot be from a bend?

As an early DFM convention, measure at least R + 2.5T from the nearest round-hole edge to the bend tangent line and R + 4T from the nearest slot edge. Because supplier guides do not always use the same bend-line reference, show the measurement origin explicitly and confirm both values against the real material, radius, V-die, bend angle, direction, sequence, and tooling.

What is the minimum slot width in sheet metal?

Use a slot width at least equal to material thickness (S >= T) as a general DFM starting point. A narrower laser-cut slot may be possible on a validated system, but pierce placement, dross, taper, heat, and narrow-web distortion need review.

When should a hole be drilled or reamed instead of laser cut or punched?

Use drilling, boring, or reaming when the hole is below the approved primary-process limit or when fit, true position, roundness, cylindricity, surface finish, or post-bend accuracy controls the part. Specify the functional requirement rather than assuming the process name guarantees it.

Need a Hole and Minimum-Feature Review Before Production?

Send ShincoFab the CAD model or drawing, material grade, actual thickness, intended process, quantity, finish, hole and slot functions, edge and bend clearances, critical tolerances, burr direction, and inspection condition. ShincoFab can review the part against available cutting, punching, forming, hardware, and secondary-process options before quotation.

Capabilities

Fabrication

Value-Added

3D Printing

Material

Products

Sheet Metal Parts

Thermal & Electrical

Sheet Metal Enclosure

Energy & Infrastructure

Industries

Resource

Why Choose Us

Capabilities

Fabrication

Value-Added

3D Printing

Material

Products

Sheet Metal Parts

Thermal & Electrical

Sheet Metal Enclosure

Energy & Infrastructure

Industries

Resource

Why Choose Us

Sheet Metal Hole Size Minimum Feature Chart

Sheet Metal Hole Size & Minimum Feature Quick Chart

How to Use This Minimum Feature Chart

Converting clear distances to drawing dimensions

Minimum Punched Hole Size by Material and Thickness

Minimum Laser-Cut Hole and Slot Size

Why supplier laser charts can be smaller than T

Hole, Slot, Edge, and Bend Clearance Rules

Hole to free edge

Between holes

Hole to bend

Minimum Slots, Notches, Tabs, and Narrow Features

Hardware, Threads, Countersinks, and Precision Holes

Self-clinching hardware

Tapped holes

Countersinks

Dowel, bearing, and locating holes

Design Checks Before Releasing a Drawing

Common Minimum-Feature Problems

What to Do When a Feature Is Below the Recommended Minimum

Download the Sheet Metal Hole Size & Minimum Feature Chart

Frequently Asked Questions

Need a Hole and Minimum-Feature Review Before Production?

Whatsapp

Address

Socials

Contact Info

Support

Get In Touch

Download the Sheet Metal Hole
Size & Minimum Feature Chart