Sheet Metal Design Guidelines

Sharing is caring

Sheet metal design guidelines are followed to design quality sheet metal enclosures. This helps in delivering the product at low cost and time. All design guidelines can not followed in one part. Therefore exceptions can be there for complex features design. In this article we will discuss sheet metal design guidelines for manufacturing parts using sheet metal press bending.

Sheetmetal are available in standard thickness. Manufacturer provide sheets thickness in gauge. But designers design sheet metal parts considering sheet thickness in mm. You can use this guide to convert sheet thickness from gauge to mm.

Sheet Metal Material Selection

Material selection is a very important part of product design. It also affects the sheet metal enclosure design. Sheet thickness and material can be selected using:

  • Simulation Studies
  • Past Experience
  • Study existing products
  • Experimental Studies

You can also use this guide to know more about sheet metal material selection.

Inside Bend Radius

Sharp inside bend radius are not recommended in sheet metal design. Because they can cause material flow problems in soft material and fracturing in hard material. Which results in localized necking or fracture.

Recommended inside bend radius for sheet metal parts should be equal to material thickness. But for harder materials ( e.g. CRCA) inside bend radius equal to 0.65 times of sheet thickness is also enough.

Bend radius throughout the sheet metal design is kept constant to take the advantage of using same tool during manufacturing.

Minimum Bend/Flange Length Guidelines

Minimum sheet metal flange bend length is maintained to avoid cracks in the bending area. It shall be equal to three times of sheet thickness plus bend radius.

Min. flange Bend length = 3X Sheet Thickness + Bend Radius

Minimum Hole Diameter Guidelines

Small sizes punch are more prone to failure during punching operation. Therefore for softer materials, recommended minimum hole diameter is equal to sheet thickness. Whereas for harder materials recommended minimum hole diameter is equal to two times of sheet thickness.

Hole/Slot Distance from Bend Edge

Minimum distance between hole/slot edge to bend edge is maintained to avoid metal distortion, deformation and fracturing.

Recommended minimum distance between hole /slot edge to bend in sheet metal design is three times the sheet thickness plus bend radius.

Center to Center Distance Between Two Holes

Minimum center to center hole distance is maintained to avoid metal distortion, deformation and fracturing.

Minimum distance between two hole center during sheet metal design should be equal to sum of hole radius plus two times the sheet thickness.

Recommended Distance = Radius of Hole1 + Radius of Hole2 + Sheet Thickness

Effect Of Grain Direction in Sheet Metal Bending

During sheet metal processing ( rolling operation), material grains are arranged in the direction of rolling.

When Sheetmetal is bend perpendicular to rolling direction grain rearranges. That has negligible effect on part strength. 

Whereas bending parallel to rolling direction can lead to cracks because of destruction in grain structure.

Bend Relief

Bend relief is provided at the end of bending edge in sheet metal design to avoid any crack tearing in the corner.

Relief height is generally kept greater than two times of sheet thickness plus bend radius.

Extrude Hole Size & Position Guidelines

Creating extruded hole using punching process requires extreme pressure/Force. Extruded hole close to the part edge can lead to sheet metal deformation or tearing. Therefore minimum distance between extruded hole to edge if maintained.

Extruded hole to part edge (B)  = 3T + D/2

Center of extruded Holes (A) =  (5 + Hole Dia + 2T)

Extruded Hole and bend edge (C) = 3T + R + D/2

Round Emboss Design Guidelines

Creating Emboss feature using sheet metal punching requires extreme pressure. Very close emboss to the part edge, can lead to deformation in the sheet metal part.

A – Distance From Emboss To part Edge = 3T + D/2

B- Distance Between Two Emboss =  (5 + D)

C- Distance between Emboss and Sheet Metal bend = 3T + R + D/2

Dimple Feature Design Guidelines

Louver Feature Design Guide

Minimum distance between louver feature and bending edge is maintained to avoid metal deformation.

(P1) Distance Between Two lowers on Shorter Edge = 5 mm

(P2) Distance Between Two lowers on Longer Edge = 8 mm

Round Knockout Design Recommendation

Minimum distance between knockout feature and bending edge is maintained to avoid metal deformation.

(P1) Distance Between Two knockout  = (5 + D) mm


To sum up,  sheet metal design guidelines are followed to ensure good quality, reduced cost and robust design. All design guidelines can not followed in one part. Therefore exceptions can be there for complex features design. We suggest you read this article on electronics enclosure design. This will give you an overview of complete enclosure design process.

Got Questions?  We will be happy to help.

If you think we missed Something?  You can add to this article by sending message in the comment box. We will do our best to add it in this post.

Sharing is caring

Add a Comment

Your email address will not be published. Required fields are marked *