Generative Sheet Metal Design Rules

Generative Sheet Metal Design Rules

Overview: Creating sheet metal parts is a metal deformation process. Because the metal is deformed rather than removed (mill or lathe), general rules help you compensate for the manufacturing process. Designing within the process parameters usually reduces tooling cost and, ultimately, the part.

Sheet Metal Tolerances

Sheet metal design is usually for parts that do not require tight tolerances. Specifying tight location and form tolerances on a sheet metal part requires additional machining operations that add additional part and tooling costs. Minimize the cost of a sheet metal part by using standard materials and material tolerances whenever possible. Tolerances should be no tighter than necessary to make the part functional.
Forming sheet metal is less accurate than other metal forming operations, such as machining or Electronic Discharge Machining (EDM); however, many parts do not require high accuracy making sheet metal forming an option. Short process time and inexpensive tooling makes forming sheet metal appealing. It's important to understand the limits in the sheet metal forming process and specify tolerances accordingly.
The forming process has three main elements:
- Blanking a flat layout.
- Bending a flange at an angle.
- Creating a radius in the bend.

Blanking a Flat Layout

When blanking a sheet to create a flat layout, the sheet can become wavy. It is important to limit the amount of waviness by specifying a flatness tolerance. Flatness is defined as all points on a surface lying on a single plane. A flatness tolerance is the deviation allowed between two parallel planes. Typical tolerances for the flatness of the blanked profile allow .005 TIR (Total Indicator Reading) for lengths up to 1 inch. For lengths from 1 to 4 inches, TIR is typically .005 per inch, and lengths over 4 inches are allowed .02 + .004 per inch of additional length.

Bending a Flange at an Angle

There are several ways to bend sheet metal. Regardless of the technique used, the typical angle tolerance for bent flanges is + 1 degree.

Creating a Radius in the Bend

The final element typical of sheet metal forming is the bend radius. The radius is generally formed with a tool or mandrel as the steel is bent around it. The actual radius is a function of compression of the material against the tool and the tension or stretching of the material on the outside. Typical tolerances used for the limits of the actual radius are based on the radius size.

Blanking Rules

Use the following rules (when possible) to blank the part in one operation. At times, parts contain features that exceed these rules making secondary tooling and operations necessary.
Consider the following when designing a part to blank:
- Open slots and tabs should never be narrower than the material thickness.
- Open slots and tabs should never be longer than five times their width.
- Convex corner radii should be at least one half the material thickness if the material is over 1/16 inch thick.
- Convex corner radii can be sharp if the material is less than 1/16 inch.

Bending Rules

When bending sheet metal, the flange being bent cannot be inside the profile. Flanges being bent must have relief on the bend radii. As the flange is bent, the material inside the bend is compressed and the material outside the bend is in tension, which causes a tear in the flange.

One solution is to move the flange away from the profile to clear the radius. Another solution is to add relief notches to allow the bend radius to compress and stretch. This latter solution is preferred because the location of the flange remains in the same place. It also preserves the design intent and you can include the relief notches in the profile or blanking tool with little additional cost or effort.
- Design flanges outside the profile.
- Use relief notches, whenever possible, to reduce the cost of tooling.
- Relief notch length should be the bend radius plus 1T minimum.
- Relief notch width should be 1T or more.
Sufficient height in the flange being bent is essential in order for the bend radius to properly form. If there isn't, adding additional material to the bending operation and then cutting it off in an additional milling operation is required which then increases operation and tooling costs in the part. Therefore, it's important to create flanges with proper height to eliminate additional operations.

- The height of the flange should be at least 2.5T plus inside bend radius for hard materials.
- The height of the flange should be at least 2T plus inside bend radius for softer materials.
The most important element when bending a sheet is the bend radius. A small inside bend radius, combined with thick material, forces the material to compress in a small area during bending. This can cause cracking, or at a minimum, severe bulging at the outside edges of the bend. If this condition is unavoidable and it causes interference with other parts, it may be necessary to modify the flat pattern or the blank to compensate for the bulge. When the bend radius is large in comparison to the material thickness or if the material is 1/16 inch or less, the bulging is usually acceptable and hardly noticeable. The following figure illustrates a flange that bulges due to a small bend radius.

Bending sheet metal with small radii can cause cracking in the bend. Cracking is a function of the inside bend radius, material thickness, and the materials hardness. The following figure illustrates a table of suggested minimum bend radii for several common materials.

Holes

Punching or piercing holes is a quick, economical way to create holes in sheet metal. It is important to remember when punching holes the physics of blanking. The material being removed is actually broken away from the parent material. The finished hole is accurate only for the first 25 to 30 percent of the hole on the punch side, the remainder of the hole is relatively rough and has a burr on the die side. If the part requires more accurate holes, punch an undersized hole and then ream to the finished size.

- A punched hole diameter must be at least the material thickness or a .062 minimum.
- For hard materials (PSI 90,000 and above), the minimum diameter must be two times the thickness.
- A + .002 hole diameter is possible for the top 25% to 30% of the hole on the punch side.
- Measure holes on the punch side for accuracy.
- Tolerance holes as minimum diameters.
- Specify burrs as a maximum allowable value.
- Call out hole locations from center of hole to center of hole.
- Determine hole location from the center of the blank, not the edge of the blank.

Feature Location

The location of a punched or blanked feature must be at least the material thickness from the edge of the blank due to the bulging that occurs as the metal is deformed.

If a hole must be close to an edge, it's recommended that you add a tab to the material or change the hole to an open slot.
The general rule for minimum distances between features or edges is the larger the feature the greater the distance. There should also be a clearance distance established for features relative to bends. The closer a feature comes to a bend, the more distortion occurs in the feature as the part is bent into shape.
- The larger the feature periphery, the farther you should stay away from other edges.
- Keep features with curved profiles 1T to 1.5T away from other edges.
- Keep features with rectangular profiles 1.5T to 3T away from other edges.
- Keep features up to 1 inch (long or diameter) 1.5T plus bend radius away from bends.
- For larger features, add an additional 1T for each inch in length.
- Features positioned relative to bends should have a location tolerance of + .01.