Sheet metal product designs begin with CAD files and in order to get the sheet metal parts or products you desire; those CAD files should follow specific sheet metal design guidelines. Placing a bend too close to a hole for example can result in fractures or deformed pieces during the sheet metal fabrication. Designing something that isn’t manufacturable is not uncommon. In fact, some research suggests that 30-50% of the manufacturer’s design time is spent correcting errors, 24% of which are related to manufacturability. So, using a Design for Manufacturing (DFM) strategy increases the chances of getting the sheet metal design right from the start, saving you both time and money.

Most custom sheet metal fabricators will tell you that tolerances are the most important factor when designing for precision sheet metal fabrication. Tolerance refers to the allowable or acceptable variation between the sheet metal design and the finished product or sheet metal part. The tolerance allows for a degree of variation that will not impact the function, structure, or general acceptability of the product. Achieving the correct tolerance is vital and can make the difference between something that aligns properly for example, and something that doesn’t.

While modern sheet metal fabrication techniques and equipment can achieve high tolerances, keep in mind that extremely tight tolerances can make a process more difficult or even impossible. Aiming for very tight tolerances can increase costs so a best practice is to design for the tightest tolerances required for the sheet metal part or product instead of the tightest tolerance achievable. There is no point in paying for a very tight tolerance if it’s not actually required for the sheet metal part.

Different processes during fabrication have different tolerances.  It’s important to understand how they impact your sheet metal design. Common tolerances are included in the table below but it's important to check with your custom fabricator to confirm their standards.

All of the numbers we’ve included in this guide are meant as sheet metal design guidelines only.  Always check with your custom fabricator to get specific tolerances from them as it varies by material type, fabricator, equipment, tools, and other factors.  Tolerances and clearances will be adjusted on a project by project basis to accommodate your needs.

Tolerances Guideline for Sheet Metal Fabrication *

May be adjusted based on part size.

There are many factors which effect actual tolerances, which reinforces the need to confirm with your fabricator before beginning your sheet metal design.

• The more processes a part undergoes, the more difficult it is to achieve tight tolerances
• The material you choose, including type and sheet thickness
• Some equipment used for sheet metal fabrication can achieve tighter tolerances than others
• Custom fabrication and assembly companies have different capabilities and equipment to accommodate tolerance requirements
• CAD designs should be created using Design for Manufacturing standards, so tolerances are realistic

Laser cutting is often a best choice for metal parts requiring precision sheet metal fabrication. Lasers can operate with tolerances from +/- 0.127mm of precision and can accommodate material up to 20 mm (0.78″) thick.

• Hole sizes are limited by the size of the laser beam
• Tapered cuts or other 3D features are not possible with laser cutting

Bending sheet metal with press brakes to achieve the desired shape. Tooling is required although not all bending processes require custom dies. The process of bending does require manual operators and different types of equipment can achieve different bend radius tolerances.

• You can’t typically achieve a true 90° corner. Corners will have radius
• Bend angles standard tolerance of ± 1°
• Bend length tolerance are typically ±0.25 mm (0.010″)

When designing for laser cutting and CNC bending processes for your sheet metal fabrication, it’s important to keep common standards top of mind for different design elements.

The sheet thickness not only determines the strength and weight of your part, but also minimum bend radii, hole and slot sizes, flange length, and other important design features. Sheet metal parts should keep a uniform thickness throughout.

Curls provide a circular roll to the edge of the sheet to provide strength and minimize exposure of the sharp edge. Unlike a hem, the edge of a curl turns in on itself. Curls can be off center or on center.

• The outside radius of a curl should be at least twice the thickness of the material being used
• Using a radius 2 times the material thickness will create a curl opening radius equal to the material thickness
• The opening of the curl should be at least equivalent to the material thickness

CLEARANCES FOR CURLS

Countersinks and counterbores are used to create a flush surface where metal parts are fastened together. A countersink creates a cone shaped hole typically designed to accommodate a screw. Counterbores however are drilled straight down and have a flat bottom, often to accommodate bolts or nuts. Neither are practical for thin materials.

• Countersinks can be no more than 0.6 times the thickness of the material
• A countersink and a fastener should have at least 50% contact

CLEARANCES FOR COUNTERSINKS AND COUNTERBORES

Hems provide strength to the hemmed edge and eliminate sharp edges but also add weight to the part. Trying to achieve a flat hem can cause fractures to the material so design for open or teardrop hems instead.

• Open hems should have an inside diameter at least equal to the material thickness. Large diameters can lose their shape.
• The return flange of an open hem should be at least 4 times the material thickness
• Teardrop hems should have an inside diameter at least equal to the material thickness
• Openings for a teardrop hem should be at least ¼ of the material thickness
• The return flange of a teardrop hem should be at least 4 times the material thickness

CLEARANCES FOR HEMS

Holes should always be designed with a diameter at least equivalent to the thickness of the material. Smaller holes can cause excessive burring and impact the life of the part. Spacing holes appropriately also helps them hold their shape during further processing steps.

• Holes and slots should have a diameter at least as large as the thickness of the material or 1.00 mm (0.04″) – whichever is greater. For alloy or stainless steel, it should be at least 2 times the material thickness.
• Materials with higher strengths require that holes and slots have a larger diameter

CLEARANCES FOR HOLES, AND SLOTS

Notches or tabs can sometimes be part of the piece itself or be intended for further bending or for joining. Notches are created by removing a section of the sheet metal from the outside edge. Tabs on the other hand are protrusions from the sheet metal edge.

• Notches must have a thickness of at least 1mm (0.04″) or equivalent to the material thickness (whichever is greater)
• The length of a straight or radius end notch should be no more than 5 times material thickness
• The length of a V notch should be no more than 2 times its width
• Tabs must have a width of at least 3.2mm (0.126″) or two times the material thickness (whichever is greater)
• Tab depth should be no more than 5 times the width of the tab
• Notch corner radius should be 0.5 times material thickness

CLEARANCES FOR NOTCHES AND TABS

Corner fillets create rounded edges to eliminate sharp corners.

• Corner fillets should be ½ the material thickness

Relief cuts can be used to prevent overhangs which are more common on thick sheet metal parts with a small bend radius. They can also help prevent tearing from bends placed close to an edge

• A relief cut should be at least equal to the material thickness in width
• Length of a relief cut should be longer than the bend radius

Welding of some materials requires preparation, including grinding, which should be considered when designing. When designing welds, using very tight tolerances minimizes the need for the welder to use wire.

• Hand welding should be for gauges greater than 20 gauge </ li>

CLEARANCES FOR WELDING

• Dimples should have a maximum diameter of 6 times material thickness
• Dimple depth should be no more than ½ the inside diameter of the dimple

CLEARANCES FOR DIMPLES

Gussets can add strength to a flange without any welding. They generally require custom tooling to produce.

CLEARANCES FOR GUSSETS

Lances involves cutting and bending on a piece without removing any material. It changes the shape and is often used to allow air flow through a part (vents and louvers).

Special tooling is often required.

• Open lances should have a minimum width of3.00mm (0.125″) or2 times the material width (whichever is greater)
• The maximum width of an open lance is 5 times the width
• Closed lances should have a minimum width of 1.60mm (0.06″) or 2 times the material width (whichever is greater)
• The maximum height of a closed lance is 5 times the material thickness at a 45° angle

CLEARANCES FOR LANCES

• The inside radius of a rib is no more than 3 times the material thickness
• Maximum depth for a round embossment or rib is equal to its inside radius
• Maximum depth for a flat embossment is equal to its inside radius plus the outside
• Maximum depth for a v embossment is equal to 3 times the material thickness

CLEARANCES FOR RIBS

*Please use these numbers as sheet metal design guidelines only and always check with your fabricator for their recommendations before completing your design.

Our team of engineers and technicians here at Komaspec have more than 15-years’ experience in sheet metal fabrication in China and are glad to review your product design together, and provide detailed design for manufacturability feedback and analysis to help you improve functionality and reduce manufacturing and tooling costs.