Design for Sheet Metal: Minimum Flange, Radius and Hole Spacing

Sheet metal is a forming process, and every forming process has geometry it cannot produce. This page lists the rules that matter when you are drawing a part that will be laser cut, bent and possibly welded: how small a flange can be, how tight a radius a bend can hold, how close a hole can sit to a bend line, and which drawing decisions quietly add cost without adding function.

Minimum Flange Height

The flange is the leg of the bend — the part that stands up off the flat. The limit is set by the tooling: the die has to fit into the space between the flange and the sheet, and if the space is too small the punch closes on material instead of bending it.

Flange Height	Verdict	What happens
Less than 1×t	Not achievable	Tooling cannot enter the space. Material tears at the corners or the bend becomes a crush.
1×t to 1.5×t	Possible, tight	Bend is supported on both sides but with little margin. Corner cracking is the normal failure mode on harder alloys.
1.5×t to 2×t	Workable	Reliable for most materials. The usual choice for functional internal stiffening flanges.
2×t and above	Comfortable	Fully supported bend. This is the right choice for visible edges, load-bearing flanges and cosmetic corners.

Rule of thumb: design at 2×t for anything a customer touches, sees or loads, and 1.5×t is an acceptable minimum for purely internal stiffening.

Minimum Internal Bend Radius

Every internal corner in sheet metal is radiused — it cannot be sharp. Metal cannot be bent to a zero inside radius without displacing an unachievable volume of material, so the die physically forms a radius. The inside radius is also the radius you see, which makes it a cosmetic decision as much as a manufacturing one.

Inside Radius	Achievable With	Notes
0.3×t to 0.5×t	Special tooling, quoted per part	Requires a punch and die pair cut for the part. Ties the part to dedicated tooling and raises cost significantly. Cosmetic use only.
1×t	Standard air bending	The industry default. Works on all common thicknesses without special tooling.
2×t to 3×t	Standard air bending	Better surface at the corner, better bend relief, and it looks better. Specify this on cosmetic parts.

The outside of the bend is not sharp either. Its radius is the inside radius plus the material thickness, so a 1×t inside radius on 3mm sheet gives you a 4mm outside radius. Increasing the inside radius improves appearance for free — there is no cost difference between 1×t and 2×t on standard tooling.

The related calculation that most often goes wrong is the flat pattern length. See bend radius and bend allowance for how inside radius drives developed length, and why two shops bending the same drawing can legitimately disagree on the flat size.

Hole-to-Edge and Hole-to-Bend-Line Spacing

Holes are the feature most sensitive to how close they sit to everything else. A hole near an edge tears out when the edge is trimmed; a hole near a bend line distorts during forming; two holes too close together pull the material between them.

Spacing Rule	Minimum	Reason
Hole centre to cut edge	1×t	Closer than this and the ligament between hole and edge tears during cutting, leaving a ragged edge that fails inspection.
Hole centre to bend line	1×t + bend radius	The hole distorts during forming. Oval holes break fastener alignment and pivot concentricity.
Hole centre to hole centre	2×t	Heat-affected zones from the two cuts merge, and the material between them distorts.
Hole centre to bend, where the hole must stay round	3×t or dimension after forming	Bend-induced stretch keeps deforming the hole. The robust fix is to machine the feature after bending.

The dimensioning trap: on a bent part, a hole dimensioned from the flat edge is a dimension in the flat condition, not the finished condition. If the hole has to stay round and in a fixed position after forming, either dimension it in the finished condition with the bend line referenced on the drawing, or move the operation to after bending. See tolerance and surface finish for how this interacts with your tolerance stack.

Hemming vs. a Flanged Edge

Both solve the problem of a raw cut edge, but they answer different requirements. A hem returns the material on itself, creating a closed, doubled edge that is safe to touch, hides the laser cut face completely, and adds real stiffness. A flange simply turns the edge up 90°.

Hemming needs extra flat length to work with: roughly one material thickness of additional allowance beyond the simple flange, and the inner radius of the hem is smaller than the outer. When you hem a 1mm edge on 2mm sheet, the inner bend is tight. That is why hemmed edges are usually specified on thinner material.

Bend Sequence and Tool Access

A part with four bends is not four independent operations. Each bend changes the geometry available to the next one, and a sequence that works on paper can leave a flange sitting exactly where the tool needs to go.

Principle	Why
Bend flange-to-flange parts in the tightest-nest order	A U-shaped channel has to close the short flanges before the long ones, or the open flanges block the punch.
Bend large radii before small ones where possible	Large bends move more material and are easier to make when the part is still flat and stable.
Keep the bend line off any hole pattern	Forming a hole on or near a bend line guarantees the hole changes shape.
Group identical bends to the same angle	Each distinct angle and radius is a tooling change. Four identical 90° bends are one setup; four different bends are four.

If a part cannot be formed in a reasonable number of setups, it is worth re-drawing. Splitting it into two parts that tab together, or moving a feature to a machined sub-component, is frequently cheaper than fighting the form.

Weld Access, Tabs and Joining Features

If the part is assembled from more than one piece, the joining method is a design decision with a cost attached. Tab-and-slot is cheapest and needs no filler, but it constrains assembly sequence and leaves visible joints. Welding is stronger and cleaner cosmetically but adds fixturing, distortion control and inspection.

Method	Use When	Design Note
Tab and slot	Enclosures, chassis, covers in thin sheet	Tab width roughly 0.8×t, slot 0.1–0.2mm wider than the tab. Slots must be positioned so the tab is inserted before the last bend where practical.
TIG / MIG weld	Structural joints, hermetic seams, thicker material	Allow for distortion and access for the torch. State whether the weld is cosmetic, structural or pressure-tight — they are very different specifications.
Self-tapping screw	Serviceable assemblies	Use on a flat land, not on a bend or near an edge. Pilot hole diameter matters; specify it rather than letting the supplier guess.
Rivet / PEM	Low-stress permanent joints	Requires flat, accessible surfaces on both sides and a minimum edge distance of about 2× diameter.

For welded assemblies the distortion discussion is on its own page — welding distortion control — because for enclosures that must seal, the weld sequence changes the part cost more than the weld process does.

Which Rules Actually Cost Money

Design Choice	Cost Effect	Why
Internal radius at 1×t or above	No cost	Standard tooling. Anything tighter is a per-part tooling charge.
Flange at 1.5×t or above	No cost	No extra operation, no risk.
Flange between 1×t and 1.5×t	Moderate	Constrains tooling and raises the scrap risk on harder alloys.
Holes at 2×t or more from edges	No cost	Standard practice; anything closer is an exception we have to review.
Machined feature on a formed part	High	A second operation and a fixturing step. Often avoidable by re-drawing.
Multiple material thicknesses	Moderate to high	Each thickness is a separate material, setup and possibly a separate supplier process.
Hemming every edge	Moderate	Extra bends, so extra setup and more flat length consumed.
One part instead of two joined parts	Usually a saving	Removes a joining operation, a fixturing step and an entire tolerance interface.

Common Drawing Mistakes

#	Mistake	Consequence	Correct Approach
1	Dimensioning a bent hole from a flat edge	Measured the wrong condition, parts rejected at final inspection	State the condition: flat or finished. Add the bend line as a dimensioned reference.
2	Zero-radius internal corner	Cannot be formed; outside corner becomes excessively large	Minimum 1×t inside radius; 2×t for appearance.
3	Flange specified as 0.8×t	Tooling interference, corner cracking, rework	1.5×t minimum, 2×t for anything functional or visible.
4	Hole 0.5×t from the cut edge	Edge tears during cutting	Keep hole centre at least 1×t from any edge.
5	No cosmetic face marked	Finish arrives on the wrong side; not recoverable	Stamp both views with the cosmetic face and grain direction.
6	Flat pattern left to the supplier	Different suppliers produce different hole positions	Specify the flat pattern if hole position after bending is critical, or dimension the finished condition instead.
7	Holes smaller than 0.5×t	Will not pierce cleanly; heavy burr on the back face	Minimum hole about 0.5×t, and roughly 1mm absolute on our machine.
8	Sealing face specified without a surface callout	Standard deburr applied, gasket will not seal	State the surface requirement (flatness, Ra, deburr or none) on the sealing face.
9	Hemmed edge on thick material	Inner radius too tight to form; edge cracks	Hem thin material, or switch to a flanged edge for heavy sections.
10	Weld described as “strong”	Supplier and buyer assume different things; possible rework	Specify structural, pressure-tight or cosmetic, plus the method and the inspection required.

Every item on this list has been found on a drawing that reached us for quotation. All of them were resolved in a short email exchange — none of them required the customer to change the function of the part.

Related Sheet Metal Pages

• Bend Radius and Bend Allowance — how inside radius becomes developed length, and the K-factor
• Sheet Metal Material Selection — choosing between cold rolled, galvanized, stainless and aluminium
• Tolerance and Surface Finish — what each process holds, and how coating changes dimensions
• Welding Distortion Control — keeping welded enclosures flat and sealable
• Sheet Metal Fabrication Service — our equipment, materials, tolerances and lead times