Sheetmetal Part

Sheet Metal Design Guidelines

Sheet metal design guidelines are followed to design quality product. 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 about the design of sheet metal parts for manufacturing using press bending.

Sheetmetal are available in standard thickness. Sheet manufacturer provide sheets thickness in gauge. But designers design products 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 very important part of product design. It also affect the product 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 parts. Because Small inside bend radius can cause material flow problems in soft material and fracturing in hard material. Which results in localized necking or fracture.

Recommended inside bend radius shall be equal to material thickness. But for harder materials ( e.g. CRCA) it can be kept 0.65 times of thickness.

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

Minimum Bend/Flange Length Guidelines

Minimum 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 Recommendation

Small sizes punch are more prone to failure during punching operation. Therefore for softer materials, recommended minimum hole diameter is equal to sheet thickness. But for harder materials it should be 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 shall be equal to 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 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), sheet metal 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. 

But 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 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 Recommendation

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 of the metal.

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

Conclusion

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 to check electronics enclosure design guidelines. 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.

Add a Comment

Your email address will not be published.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