Metal stamping design guidelines help engineers create parts that can be manufactured consistently without unnecessary tooling complexity, material distortion or secondary machining.

The most important principle is to design features in relation to the material thickness. Hole size, edge distance, bend radius, flange height and notch width are all influenced by the thickness and mechanical properties of the selected sheet metal.

Following practical design-for-manufacturing principles can reduce cracking, burr formation, tool wear, dimensional variation and production costs before a stamping die is manufactured.

What Is Metal Stamping?

Metal stamping is a manufacturing process that converts flat sheet metal or coiled strip into a specific shape using presses, punches and dies.

Depending on the component, the stamping process may include:

Blanking
Piercing
Punching
Bending
Embossing
Coining
Flanging
Progressive die stamping

Simple parts may require only one stamping operation. More complex components can pass through several forming stations inside a progressive die before the finished part is separated from the strip.

Successful production depends not only on the stamping equipment but also on the design of the component. Small changes to hole positions, bend radii or tolerances can significantly affect tool life, part quality and total production cost.

Quick Metal Stamping Design Reference

In the following guidelines, T represents material thickness and R represents the inside bend radius.

Design feature	Recommended starting point
Minimum hole diameter in ductile material	At least 1.2T
Minimum hole diameter in harder material	Approximately 1.5T–2T
Minimum slot width	At least 1.5T
Hole-to-edge distance	At least 2T
Hole-to-bend distance	Approximately 2.5T + R
Inside bend radius	At least 1T
Minimum flange or bend height	Approximately 2.5T + R
Minimum notch or tab width	At least 1.5T
Typical bend-angle variation	Approximately ±1°
Expected burr height	Up to approximately 10% of T

These values should be treated as initial design rules rather than guaranteed tolerances. Material strength, temper, grain direction, tooling strategy, part geometry and production volume can all influence the final requirements.

Holes and Slots in Stamped Parts

Holes and slots are normally produced by piercing. A punch pushes the sheet metal against a die opening until the material first deforms, then shears and finally fractures.

Because of this process, a stamped hole does not normally have the same wall condition as a drilled or reamed hole. The upper section often contains a smooth burnished area, while the lower section contains a fracture zone and a small burr.

This wall profile is usually acceptable for clearance holes, ventilation openings, locating features and many assembly applications. A secondary machining operation may be necessary when the hole requires a highly uniform wall, a very tight diameter or an accurate bearing surface.

Minimum Hole Diameter

For relatively ductile materials, the hole diameter should generally be at least 1.2 times the sheet thickness.

Harder materials, including some stainless steels, spring steels and heat-treated alloys, may require a larger minimum diameter. Using a diameter of approximately 1.5 to 2 times the material thickness can reduce punch stress and premature tool failure.

Smaller holes may still be technically possible, but they usually require specialised punches, more frequent tool maintenance or secondary operations.

Minimum Slot Width

A practical starting point for slot width is approximately 1.5 times the material thickness.

Very narrow slots create thin and fragile punch sections. These tools are more likely to deflect, wear or break during production, particularly when stamping harder or thicker materials.

Whenever possible, use wider slots, rounded slot ends and standardised dimensions.

Distance Between a Hole and an Edge

Place holes at least two material thicknesses away from the nearest part edge.

When a hole is too close to an edge, the remaining material may not provide enough support during piercing. This can cause the edge to bulge, tear or become dimensionally unstable.

Increasing the edge distance can improve hole quality and reduce the need for trimming or secondary machining.

Distance Between Holes and Bends

Holes and slots located close to a bend can stretch or become oval during forming.

As a general starting point, keep the edge of a hole at least 2.5 times the material thickness plus the bend radius away from the bend line.

Long slots and unusually large openings may require additional spacing. The forming direction, bend angle and material properties should also be reviewed before tooling begins.

Designing Bends and Formed Features

Bending places the outer surface of the sheet in tension while compressing the material on the inside of the bend. Poor bend geometry can cause cracking, excessive springback, tearing or unstable angles.

Select a Suitable Bend Radius

For many stamped components, an inside bend radius equal to the material thickness is a practical starting point.

A smaller radius may be possible with soft and ductile materials. However, harder materials and high-strength alloys generally require a larger bend radius to reduce cracking.

The selected radius should be evaluated together with the alloy, temper, thickness and required bend direction.

Consider the Material Grain Direction

Rolled sheet metal has a grain direction created during material production.

Whenever practical, critical bends should run across the grain rather than parallel to it. Bending parallel to the grain can increase the risk of cracking, especially in harder, tempered or high-strength materials.

The required grain orientation should be identified on the engineering drawing when it is important to part performance or forming reliability.

Provide Enough Flange Height

The flange must contain enough material to be held and formed consistently by the tooling.

A common starting point for minimum flange height is:

Minimum flange height = 2.5T + R

Shorter flanges may require special tooling, additional forming stages or a different manufacturing method.

Add Bend Relief Where Necessary

A bend relief is a small cut or opening positioned beside the end of a bend. It separates the material being formed from an adjacent flat area.

Without sufficient relief, compressed material may tear, twist or bulge into the surrounding surface.

A practical relief can be designed with a width of approximately two material thicknesses and a length equal to the bend radius plus the material thickness. Actual requirements may vary depending on the bending method and part geometry.

Rounded or obround reliefs can also help reduce stress concentration compared with sharp rectangular corners.

Dimensioning and Tolerancing Stamped Parts

Stamped features behave differently from machined features, so drawings should reflect the actual manufacturing process.

For blanked, punched and pierced edges, dimensions should account for the burnished area, fracture zone and natural taper created by shearing.

Inside dimensions are generally evaluated from the shortest part of the sheared profile, while outside dimensions are evaluated from the longest part. The measurement method should be agreed with the manufacturer when the sheared edge is functionally important.

For formed components, dimensioning to the inside of a bend is usually more stable than dimensioning to the outside.

Account for Bend-Angle Variation

A formed 90-degree bend may commonly have an angular variation of approximately ±1 degree unless tighter control is required.

The effect of this variation becomes greater as the distance from the bend increases. A hole positioned far from the bend line may therefore show more positional variation than a feature located close to it.

Parts containing several bends must also account for tolerance accumulation. Each bend angle, flange length and forming operation contributes to the final dimensional result.

Avoid Unnecessary Tight Tolerances

Tight tolerances should be applied only to features that affect assembly, sealing, alignment, safety or functional performance.

Over-tolerancing can lead to:

More complex dies
Additional die stations
More frequent tool adjustment
Increased inspection requirements
Secondary machining
Higher scrap rates
Greater production cost

Use general stamping tolerances for non-critical geometry and clearly identify the dimensions that are essential to the function of the component.

Tabs and Notches

Tabs and notches are frequently used for positioning, joining, locating and assembly.

As a general rule, their width should not be less than approximately 1.5 times the material thickness.

Very narrow tabs can bend or break during stamping and handling. Narrow notches also require thin punch sections that may wear quickly or fail under repeated loading.

Rounded internal corners are preferable because they distribute stress more evenly and are easier to produce with durable tooling.

Corner Radii

Sharp external and internal corners increase stress concentration and can make stamping tools more difficult to manufacture and maintain.

Where the component function permits, add a radius to every corner of the blank. A minimum radius of approximately half the material thickness can be used as an initial design target for many flat stamped parts.

Larger radii are generally easier to stamp and can improve material flow during forming.

Sharp corners may be possible in thin materials, but they should be specified only when they are necessary for the part’s function.

Burr Direction and Burr Control

Burrs are a normal result of blanking and piercing. They form on the exit side of the material where the final fracture occurs.

Burr height can reach approximately 10% of the sheet thickness under typical stamping conditions, although the actual result depends on tool clearance, material properties, punch condition and maintenance.

The drawing should identify the acceptable burr direction when it affects:

Assembly
Electrical contact
Sealing surfaces
Operator handling
Sliding components
Cosmetic appearance
Coating application

Burrs can be reduced through correct punch-to-die clearance, tool maintenance and suitable corner geometry. Deburring, tumbling, brushing or secondary finishing may be required when sharp edges are not acceptable.

How to Reduce Metal Stamping Costs

The most effective cost reductions are usually made before the die is built.

To improve manufacturability:

Use standard material grades and available sheet thicknesses.
Base minimum feature sizes on material thickness.
Keep holes and slots away from edges and bends.
Use generous internal and external radii.
Avoid extremely narrow tabs, slots and notches.
Apply tight tolerances only to functional dimensions.
Specify burr direction and grain direction where necessary.
Review the component with the stamping supplier before finalising the drawing.
Confirm annual volume before selecting progressive, transfer or single-operation tooling.
Allow the manufacturer to perform a formal DFM review before tool production.

A small geometry adjustment can prevent repeated die modifications, additional production stages and expensive secondary machining.

Frequently Asked Questions

What is the minimum hole size for metal stamping?

A common starting point is a hole diameter of at least 1.2 times the material thickness. Harder materials may require a diameter of approximately 1.5 to 2 times the thickness.

How close can a stamped hole be to an edge?

The distance from the edge of the hole to the edge of the part should generally be at least two times the material thickness.

How far should a hole be from a bend?

A practical starting distance is approximately 2.5 times the material thickness plus the inside bend radius. More space may be required for long slots or severe forming operations.

What is a suitable bend radius for stamped sheet metal?

An inside bend radius equal to the material thickness is a common starting point. Harder or less ductile materials may require a larger radius.

Are burrs acceptable on stamped parts?

A limited burr is normally expected after blanking or piercing. The drawing should specify burr direction, maximum acceptable burr height and whether deburring is required.

Final Design Recommendation

Good stamped metal part design balances function, manufacturability, tooling life and production cost.

Use material thickness as the basis for hole sizes, edge distances, bend radii, flange heights and notch dimensions. Avoid unnecessarily sharp geometry and apply demanding tolerances only where they directly support the function of the component.

Before approving production tooling, submit the 2D drawing, 3D model, material specification, sheet thickness, annual quantity and critical inspection requirements for a complete stamping DFM review.