Sheet Metal Design Guidelines : How to Design Good Sheet Metal Parts

Sheet metal design guidelines are followed to design quality sheet metal enclosures. This helps in delivering the product at low cost and faster timelines. All sheet metal design guidelines are very difficult to follow in complex sheet metal parts.

Therefore exceptions can be there for complex sheet metal parts. But testing these exceptions before design release is always a good practice. In this article we will discuss sheet metal design guidelines for manufacturing sheet metal parts using a press bending machine.

Following points should be considered during the design of sheet metal parts for press bending.

Sheet Metal Material Selection

Sheetmetal are available in standard thickness. Manufacturer provide sheets thickness in gauge. But designers design sheet metal parts considering sheet thickness in mm. Material selection is a very important part of product design. It has impact on sheet metal part design as well. Sheet thickness and material selection can be done in the following ways.

  • Simulation Studies
  • Past Experience
  • Reverse Engineer existing products
  • Experimental Studies

Read this guide to know more about sheet metal material selection Process.

Minimum inside bend Radius for Sheet Metal Parts

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.

Sharp inside bend radius in sheetmetal parts can cause material flow problems in soft material and fracturing in hard material. Which results in localized necking or fracture. Therefore sharp bend radius is not recommended in sheet metal parts.

Recommended sheet metal inside bend radius is equal to material thickness.
Recommended inside bend radius in Sheet Metal

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

Minimum Sheet Metal Bend Length Recommendations

Minimum sheet metal flange length shall be equal to three times of sheet thickness plus bend radius.
Minimum Recommended Sheet metal Bend Length

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

Minimum Sheet Metal Flange Bend Length = 3 x Sheet Thickness + Bend Radius

Minimum Hole Diameter Guidelines

for softer materials, recommended minimum hole diameter is equal to sheet thickness.
Minimum Hole Diameter in sheet metal

Small sized punches are more prone to failure during sheetmetal punching operation.  Therefore for softer materials, the 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

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

Minimum distance between hole/slot edge to bend edge is recommended to avoid metal distortion, deformation and fracturing. Recommended minimum distance between hole /slot edge to bend in sheet metal parts is three times the sheet thickness plus bend radius.

Center to Center Distance Between two Holes

Minimum center to center distance between two holes in sheet metal parts is required 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 Center distance between holes in Sheet Metal Part

Recommended Minimum distance between two hole centers in 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

When Sheetmetal is bend perpendicular to rolling direction grain rearranges. That has negligible effect on part strength.
Grain Orientation in sheet metal Parts

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

Bend Relief in Sheet Metal Bend

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

Bend relief is provided at the end of the 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 and Position Guidelines

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

This Image shows the recommendation for extruded hole in sheet metal

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 in Sheet Metal Parts

Louver Feature Design in Sheet Metal

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 be 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 the complete enclosure design process.

We will keep adding more information on sheet metal design guidelines. Please write to us if you need any support in sheet metal part design.

2 Responses

Add a Comment

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