Sheet Metal Design: Flanges, Bends, and Flat Patterns

Sheet Metal Design in SolidWorks: Flanges, Bends, and Flat Patterns

Sheet metal fabrication is central to both manufacturing and marine industries. Electrical enclosures, duct work, brackets, and equipment housings are routinely formed from flat stock that is cut, punched, and bent into shape. SolidWorks provides a dedicated Sheet Metal module that lets you model the finished 3-D part and then unfold it into a flat pattern — the actual shape that will be cut before bending.

Starting a Sheet Metal Part: Base Flange Method

The most common way to begin a sheet metal part is the Base Flange / Tab tool. You sketch the profile of the first flat face, then assign a material thickness and default bend radius. SolidWorks stores these settings in the Sheet Metal feature at the top of the Feature Manager tree, so all subsequent features inherit them unless you override individually.

An alternative starting point is Convert to Sheet Metal, used when you already have a solid body (perhaps imported from another CAD system). You select faces to remove and edges to become bends. Both methods reach the same goal; for original designs, Base Flange is simpler and preferred.

Adding Flanges

• Edge Flange — adds a bent tab along any straight edge of the existing sheet metal body. You set the flange angle, length, and position (material inside, outside, or tangent to the bend). Edge Flange is the workhorse for enclosure walls.
• Miter Flange — sweeps a flange profile along a chain of edges, automatically cutting miter joints at corners so adjacent flanges meet cleanly. It is ideal for multi-sided lips or channels.
• Hem — folds the edge back on itself to create a safe, finished edge or a stiffened lip. Common hem types are Open, Closed, Teardrop, and Rolled. In marine applications, closed hems on aluminum or stainless enclosures prevent corrosion-trapping crevices and eliminate sharp edges that can cut wiring.

Bend Allowance and K-Factor

When metal bends, the outer surface stretches and the inner surface compresses. Somewhere through the thickness is a layer that neither stretches nor compresses: the neutral axis. The K-factor defines where this neutral axis sits as a fraction of the material thickness (K = neutral axis distance ÷ thickness). A K-factor of 0.5 means the neutral axis is at the mid-thickness.

The bend allowance (BA) is the arc length along the neutral axis through the bend:

```

BA = π × (IR + K × T) × (θ / 180)

```

Where:

• IR = inside bend radius (inches)
• T = material thickness (inches)
• K = K-factor (dimensionless)
• θ = bend angle in degrees

For 90° bends this simplifies to:

```

BA = π/2 × (IR + K × T)

```

The flat blank length for a part with two 90° bends equals the sum of the flat legs plus both bend allowances:

```

Blank = Leg1 + BA1 + Leg2 + BA2 + Leg3

```

K-factor values are material- and process-dependent. Typical published values for mild steel are around 0.33–0.44; for 304 stainless steel (common marine grade), published fabrication references often cite values near 0.38–0.45 depending on tooling. Always confirm with the material supplier or your shop's bend test data — SolidWorks lets you enter the exact K-factor in the Sheet Metal feature so the flat pattern matches your floor.

Flat Pattern and Drawing

Once the 3-D model is complete, click Flatten (or toggle the Flat Pattern feature at the bottom of the Feature Manager tree). SolidWorks unfolds every bend simultaneously and shows the flat blank with bend lines displayed as dashed lines.

To document the flat pattern:

1. Create a new drawing and insert a Flat Pattern view (available in the View Palette for sheet metal parts).

2. Use Insert → Sheet Metal → Bend Notes to place the bend direction, angle, and radius annotations on each bend line.

3. Add overall dimensions for the blank length and width.

4. Verify these dimensions match your hand calculation. If they do not agree within your tolerance, check the K-factor, the inside bend radius, and whether any flange lengths were measured from the correct reference (inside or outside).

Material and Gauge Considerations

14-gauge stainless steel (Type 304 or 316L for marine) has a nominal thickness of approximately 0.0781 in. (1.984 mm) per standard gauge tables. Always confirm actual thickness from the specification sheet — gauge-to-inch conversions vary by metal type (steel gauge tables differ from aluminum gauge tables).

Safety in the Sheet Metal Shop

Shop safety applies even though this lab is CAD-based. When you move your design to fabrication:

• PPE: Cut-resistant gloves when handling sheet stock; safety glasses at all times near shearing and punching equipment.
• Sharp edges: Never slide bare hands along cut sheet edges. Deburr before handling.
• Press brakes: Never reach into a press brake during a stroke. Lockout/Tagout (LOTO) procedures per OSHA standards must be followed before clearing jams or adjusting tooling.
• Housekeeping: Metal shavings and slugs from knockouts are slip and cut hazards — clean the work area after each operation.

In CAD, model bend radii that are realistic for your tooling — too-small radii cause cracking in stainless steel and are a fabrication safety concern, not just a quality issue.