SolidWorks Sheet Metal Modeling: 8 Expert Techniques for Fabrication-Ready Designs

1. Always start in the sheet metal module (not the standard part environment)

You can save yourself from mistakes like designing any feature, which won’t generate flat patterns downstream by first assigning the component as a sheet metal part in SolidWorks. To do this in the right way, select Insert > Sheet Metal > Base Flange/Tab and launch the module. This makes SolidWorks load properties specific to sheet metal, including material thickness, bend radius defaults, and relief types, making it easier for the designer to work with thin plates and sheets.

If you begin working in the standard SolidWorks environment and not in the sheet metal module, then you will have to face flat pattern errors and rework later when you try to convert. The sheet metal module ensures your design carries accurate bend information from the very first sketch, whether you add edge flanges, miter flanges, hems or tabs or any other feature.

Sheet Metal Module in SolidWorks

When to use the weldments module alongside sheet metal

The Weldment module offers preloaded profiles so you can automatically generate machined part and welding part configurations from your 2D and 3D sketches. So it’s convenient to use the module in parallel with the sheet metal module if your assembly includes welded structural members such as frames, supports, or enclosures. Also, the design table helps you to store and reuse hundreds of configurations of things like structural channels and tubes from your CAD library.

Configurable Custom Weldment Profiles in SolidWorks

2. When to convert a solid body to sheet metal — And how to do it without errors

It is not a fixed practice to always start a feature or part directly in the sheet metal module. Items like hoppers for SPMs, HVAC ductwork, or transition pieces, that have complex geometries, are usually modeled first as solid bodies or surfaces, and then converted. For this, you use the Insert > Sheet Metal > Convert to Sheet Metal workflow.

Sheet Metal Options in SolidWorks

Especially for non-standard shapes, you can reduce time and complexity when you adopt this approach, as this cuts down the total modeling steps you’d otherwise need to take. So, for example, when designing a hopper it is easier to first model it in the standard environment in SolidWorks and then convert the solid part to the required thickness using the shell function. It would take many steps to do the same if you had designed the hopper in the sheet metal module from start. Keep in mind, however, that conversion to sheet metal will work smoothly only if you make sure that no internal fillets clash with the bend radius, and all faces of the part have the same thickness.

Complex Sheet Metal Designs

Sheet Metal Designs

3. How to set K factor and bend allowance in Solidworks for accurate flat patterns

The cutting accuracy of CNC press brakes and laser cutters is controlled by the accuracy with which the flat patterns reflect the part’s unfolded size. And this flat pattern accuracy is determined in turn by the K-factor set by the designer. In SolidWorks sheet metal environment, the K-factor is represented by a simple formula K = t / T, with t being the neutral axis and T being the thickness of the material. So the K factor fixes the ratio of the distance from the inside face of a bend to its neutral axis, divided by material thickness.

Sheet Metal Understanding K Factor

Typical K factor values by material

Once you set the K factor, SolidWorks will take that input and auto calculate flat patterns for each bend. You start this in the Sheet Metal Parameters panel and go to the Bend Allowances. Here you will find a dropdown menu where you select K-factor and then enter the value. If your fabrication shop has preset values, you can provide them instead to put into the Bend Allowances or Bend Deduction fields.

Sheet Metal Parameters

Bend Allowance vs. Bend Deduction: Both of these values are used and needed for accurately building flat patterns. However, preferring one over the other depends on the press brake calibration data of individual fabrication shops. While Bend Allowance gives the arc length of the neutral axis between bend lines, Bend Deduction gives the difference between the actual length of the flat pattern and the total of outside dimensions.

4. Use gauge tables instead of manual thickness entry

Entering thickness values for each part by hand is a recipe for errors and inconsistencies because individual designers can use different values. To avoid such errors, we use Gauge Tables in SolidWorks and standardize part values and validate against uniform data. This ensures the material thickness, bend allowance/deduction and bend radius for the part is uniform across design and fabrication.

In most workshops, the fabrication teams build custom gauge tables in Excel to match the shop capacities and standards, though SolidWorks does come with a default set of gauge tables for common materials. The shared custom gauge table provides the source of truth for all designers and fabricators and prevent inconsistencies in thickness and flat pattern errors. It is stored in a shareable location with access for those working on the job. You set up the gauge table under the Sheet Metal feature by selection the ‘Use gauge table’ option.

5. Build large assemblies using top-down parametric modeling

For large sheet metal assemblies, it is good to first create a master layout sketch and define all key reference planes and assembly dimensions. This helps you to fully use SolidWorks’ top-down modeling and save time. Team members can refer to and link the master layout when designing any individual part. And this ensures all related parts are updated whenever there is any change in even a single parameter in any part across the project. This makes large sheet metal assemblies work smoothly as you do not have to worry whether changing a single parameter, say the overall enclosure width, would lead to mismatches and misses.

Sheet Metal Exercise in SolidWorks

With the top-down approach accommodating multiple client design revision requests cease to be a problem. As you don’t need manual updates for the dozen of parts and drawings for each change, response becomes faster on all fronts. Hardware insertion, like placing fasteners into holes, also speeds up with drag-and-drop and auto-snap freeing you from the need to keep clicking in sequence over and over.

6. How symmetry and CNC coordinate alignment reduces material waste

Set the model origin in SolidWorks to match the CNC cutter or press brake’s home position before you begin modeling. For correct fabrication, the coordinates of your CAD model must match that of the target CNC machine. For this, you need to set your model origin in SolidWorks against the CNC cutter or press brake’s home position, and only then start work. This will ensure your digital sheet metal models are good enough to support direct manufacturing.

By using symmetry from the beginning of the design process you can greatly reduce modeling time and material waste. Use mirror features and symmetric mates in assemblies to make sure the parts are evenly balanced. With symmetry as your key approach, you can optimize nesting better during fabrication because you can rotate and pack symmetric flat patterns on the raw sheet stock more efficiently. Center-based symmetry also provides more manufacturing flexibility downstream and prevents rework.

7. Leverage forming tools for louvers, lances, and embossed features

Very common sheet metal deformations and parts like louvers, lances, dimples and embossing features are carried out using the forming tools in SolidWorks. You simply drag a tool from the Design Library onto a sheet metal face and apply the deformation. However, there are two things to know about this workflow. You need to use the Position tab to place the tool at the correct insertion point and press the Tab before releasing the drag.

The first step ensures the tool does not float undefined but is placed at punch location properly, and the second step helps to flip or rotate the tool to punch from the correct side or direction.

The tool automatically adjusts to the material thickness and updates the flat pattern. But keep in mind that actually the tool deformation geometry is set by the punch model itself. What adjust to that geometry are the flat pattern representation and how the inside radius behaves in relation to the thickness. If your inside bend radius on the forming tool is smaller than what it should be given the material thickness, the tool will fail or end up with invalid geometry.

For custom forming tools, model the die geometry and define the stopping face using the Forming Tool command on the Sheet Metal tab, then save as .sldftp file. Without a defined stopping face, the depth of the deformation is undefined and the tool is unusable, and defining Faces to remove clarifies about the openings. If you are using legacy .sldprt files, then at the beginning of work you also need to right-click and designate the Design Library folder as a Forming Tools Folder, otherwise the drag and drop will fail to work. This allows your team to reuse proprietary punch geometries by ensuring the flat pattern accurately reflects the manufactured part, with all formed features.

8. Validate flat patterns before sending to fabrication

Before you think of exporting flat patterns for laser cutting or CNC punching, you need to validate them in SolidWorks using the Flatten feature. Be sure to check that all bends unfold without issues, none of the faces overlap, and your bend calculations match overall dimensions. Once these checks are done, you can safely export the flat pattern as a DXF file. For this, select the “Flat pattern geometry” option and click File > Save As > DXF.

You need to set up routine verification checks to run before exporting the DXF file. This increases accuracy and much reduces rework and scrap. Common flat pattern validation checks used for these checks include verifying the positioning of bend lines and ensuring that the relief cuts are proper for the given material thickness. You also need to be sure that the flat pattern boundary and the expected unfolded dimensions match each other.