How to Flatten Surface in SOLIDWORKS?

In sheet metal design, a flattened surface (or flat pattern) is what the manufacturing team actually cuts and forms.
Laser cutting, punching, nesting, estimating material usage, and creating shop drawings all rely on an accurate flat pattern generated from the 3D model.

SOLIDWORKS calculates this flat pattern automatically for sheet metal bodies and lets you toggle between the formed and flattened states with a single command.
Understanding how to control the Flat-Pattern feature and its options is essential if you want the flat layout to match what comes off the press brake.

Sheet Metal Flat Pattern vs. General Surface Flattening

This article focuses on sheet metal parts, where SOLIDWORKS creates a Flat-Pattern feature that can be unsuppressed or controlled with the Flatten command.
For non–sheet metal models (for example, complex formed plastic or imported STEP geometry), SOLIDWORKS also provides a separate Surface Flatten command on the Surfaces tab, which can flatten a selected surface and then be thickened or converted to sheet metal if needed.

Why do we need a flattened surface?

From a manufacturing point of view, the flat pattern is used to:

• Generate DXF/DWG files for laser, plasma, waterjet, or punching machines.
• Check overall blank size, material utilization, and nesting layouts.
• Place bend lines and notes on drawings for the press brake operator.
• Estimate weight and cost based on material area and thickness.

SOLIDWORKS calculates the developed length of each bend using bend calculation methods such as K-Factor, Bend Allowance, or Bend Deduction, often driven by gauge/bend tables that match your shop’s tooling and material. Choosing realistic values here is crucial for the flat size to be accurate.

Example: Breaker bracket sheet metal part

Assume we have the breaker bracket below that needs to be manufactured as a sheet metal part. The 3D model is already created using SOLIDWORKS Sheet Metal tools.

Method 1: Unsuppress the Flat-Pattern feature

When you create a sheet metal body (for example with Base Flange/Tab or Convert to Sheet Metal), SOLIDWORKS automatically adds a Flat-Pattern feature near the bottom of the FeatureManager design tree.
By default, this feature is suppressed while you work on the formed model.

To flatten the part using this feature:

1. Open your sheet metal part (the breaker bracket in this example).
2. In the FeatureManager design tree, scroll to the bottom until you see the Flat-Pattern folder or feature.
3. Right-click Flat-Pattern and choose Unsuppress.

Once unsuppressed, the Flat-Pattern feature activates the flattened state of the part.

The model is now shown as a flat layout, with bends unfolded according to your sheet metal parameters and bend tables.
In this state you can measure the blank size, export DXF/DWG, or create flat pattern drawing views.

Method 2: Using the Flatten command on the Sheet Metal tab

Instead of manipulating the Flat-Pattern feature directly, you can also use the Flatten command on the Sheet Metal tab. This is often faster and is the recommended way to toggle between folded and flat states.

To use the Flatten command:

1. Make sure the Sheet Metal tab is visible in the CommandManager (right-click the tabs area and enable it if needed).
2. With your sheet metal part active, click Flatten on the Sheet Metal toolbar.
3. Click Flatten again to return to the formed (folded) state.

The Flatten command simply toggles the suppressed/unsuppressed state of the Flat-Pattern feature behind the scenes, so both methods produce the same result.

Editing the Flat-Pattern feature

Flattening is not just an on/off switch. The Flat-Pattern feature has several options that affect how the flat layout is displayed and how corner and bend details are handled.
You can access these options by right-clicking Flat-Pattern in the FeatureManager tree and choosing Edit Feature.

1. Fixed face

The first key option is the Fixed face. This is the face that stays stationary while the rest of the model “unrolls” around it during flattening. In practice, this usually corresponds to the face that sits on the press brake bed or a main mounting surface in the assembly.

To set or change the fixed face:

1. In the Flat-Pattern PropertyManager, locate the Fixed face selection box.
2. Click inside the box, then pick the face you want on the model.
3. Click OK to rebuild the flat pattern.

Choosing a consistent fixed face is important because it affects how the flat pattern is positioned in drawings and exported DXF files, which in turn impacts how the shop nests and locates the part on the machine.

To change the fixed face later, simply reopen the Flat-Pattern feature, clear the current face, and click a new one.
SOLIDWORKS will update the flat layout using the new reference.

2. Merge faces

The Merge faces option controls whether planar faces that are coincident in the flat pattern are merged into one large face, or kept separate with visible edges where each bend unfolds.

If Merge faces is checked, SOLIDWORKS merges planar and coincident faces in the flat pattern so that no edges are shown in the bend regions. This produces a very clean outline of the blank and is ideal when you only care about the outer profile for cutting.

If Merge faces is unchecked, the flat pattern keeps the internal edges where bends meet, which makes it easier to see bend locations, tangent lines, and transitions.
This is useful for inspection, manual layout, or when you want bend lines to show up clearly in drawings.

3. Simplify bends

The Simplify bends option straightens curved edges in the flat pattern. When it is enabled, SOLIDWORKS replaces complex curved bend edges with simpler straight segments in the flattened state. When it is disabled, the true curved edges are preserved.

Reasons to enable Simplify bends:

• Generate a simpler profile for processes that don’t require exact curvature (for example, manual layout or basic CNC routing).
• Reduce file complexity and speed up certain operations when very detailed curvature is not needed.

Reasons to leave it off:

• You want the flat pattern to represent the true developed geometry for precise laser cutting or tight-tolerance parts.
• You need accurate edge lengths for downstream processes such as forming simulations or inspection templates.

4. Show slit

The Show slit option controls whether SOLIDWORKS displays small relief slits that may be automatically added in tight corner regions. When enabled, the slit appears in the flat pattern as an extra cut that helps avoid overlapping material in corners.

In scenarios where the flange extension or corner geometry would otherwise leave overlapping material at the bend, SOLIDWORKS can introduce a slit as part of the flat pattern to meet bend relief rules and prevent tearing.
If you clear Show slit in the Flat-Pattern PropertyManager, the extra relief cut is removed from the flat pattern display, which may be desirable if your shop handles these reliefs manually or uses different corner practices.

5. Corner treatment

The Corner treatment checkbox applies automated treatments to sheet metal corners so that the flattened part has cleaner, manufacturable corner conditions.
This works together with Corner Relief and bend transition settings to remove overlaps and define consistent gaps between flanges.

Typical reasons to keep Corner treatment turned on include:

• Ensuring that adjacent flanges do not overlap in the flat pattern.
• Automatically creating appropriate corner reliefs for the material and tooling.
• Producing cleaner DXF/DWG geometry for CNC cutting.

In some special cases—such as when you already modeled custom corner features—you may turn it off to prevent SOLIDWORKS from adding additional relief cuts. You can control the default behavior for new parts via Tools > Options > Document Properties > Sheet Metal, then update your part template.

Getting accurate flat patterns: bend calculation basics

Flattening is only as accurate as the bend parameters behind it. SOLIDWORKS offers three main bend calculation modes:

• K-Factor – Locates the neutral axis as a fraction of the material thickness. This is often calibrated from shop test bends for each material, thickness, and tooling combination.
• Bend Allowance – Specifies the extra arc length added in the bend region compared to a simple “net” length between bend lines.
• Bend Deduction – Specifies how much to subtract from the sum of flange lengths to determine the flat length.

SOLIDWORKS can store these parameters in gauge/bend tables, which associate bend allowance, radius, and K-factor with specific thicknesses and materials. Using tables that match your fabricator’s real-world values is one of the most effective ways to ensure that your flattened size matches the formed part.

Flattening non–sheet metal surfaces with Surface Flatten

The title of this article mentions “surface” for a reason: sometimes you’re working with geometry that is not yet a sheet metal body—such as imported surfaces, complex formed shapes, or STEP files from another CAD system.

In these cases you can use the Surface Flatten command (on the Surfaces tab) to select a surface and generate a flattened representation. This is especially useful when:

• You receive a non-sheet-metal model and need a quick flat pattern.
• You want to study deformations on a complex surface or map decals or patterns onto it.
• You plan to thicken or convert the flattened surface to sheet metal later.

Keep in mind that Surface Flatten works differently from the Sheet Metal flat pattern and may not always correspond directly to what you can form on a press brake. For production sheet metal parts, it is usually better to use true Sheet Metal features whenever possible.

Practical tips and troubleshooting

Use Sheet Metal features or Convert to Sheet Metal

Start your design as a sheet metal part using Base Flange/Tab, or convert a solid body using the Convert to Sheet Metal tool, which lets you specify thickness, bends, and rips so the part can be flattened.

SOLIDWORKS sheet metal generally prevents you from creating features that cannot be flattened; if a feature would break the flat pattern, you’ll see errors in the FeatureManager and the flat pattern may fail or look incomplete.

Edit in the flat state with Unfold/Fold when needed

While the Flatten command is convenient, for certain operations it is better practice to use the Unfold and Fold commands:

• Use Unfold to temporarily flatten selected bends relative to a fixed face.
• Add holes, cuts, or other features in the flattened state.
• Use Fold to return the bends to the formed state, carrying your new features with them.

This approach ensures edits are correctly reflected in both the flat and formed configurations and is often recommended over editing directly in the Flat-Pattern configuration.

Watch out for zero-thickness and non-manifold geometry

Errors like “zero-thickness geometry” or non-manifold edges can prevent a sheet metal part from flattening correctly. These occur when there is effectively no material between adjoining faces or edges (for example, when a cut or overlap leaves zero thickness).

If your flat pattern fails to rebuild:

• Temporarily suppress recent features one by one and try flattening again to identify the problematic operation.
• Check that cuts intersect bends correctly and that you are using Normal cut where appropriate.
• Review bend deductions/K-factor values if you have recently changed material or tooling settings.

Summary

Flattening a sheet metal part in SOLIDWORKS is straightforward once you understand how the Flat-Pattern feature, Flatten command, and property options work together.
Use the Flat-Pattern feature or Flatten button to toggle between formed and flat states, set a logical fixed face, and fine-tune Merge faces, Simplify bends, Show slit, and Corner treatment to match your manufacturing needs.
Combine these tools with accurate bend calculation data (K-factor, bend allowance/deduction, and gauge tables) and, where necessary, the Surface Flatten command for non–sheet metal surfaces, and you’ll consistently produce flat patterns that match how your parts are cut and formed on the shop floor.