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SolidWorks Convert Solid to Sheet Metal: V-Shaped Reinforcement Sheet Metal Part Unfolding Tutorial

Table of Contents

In today’s post, we’ll use a real-world customer case—a 3mm-thick steel plate measuring 500×340 with an internal V-shaped reinforcement structure—to walk you through the process of successfully fabricating it using the approach of “first disassemble the part, then unfold each section separately, and finally reassemble it.”

As long as you follow along step by step, you’ll be able to apply this same method to similar bent and welded parts in the future.

Case Background

This is the drawing provided by the client.

The client sent an engineering drawing (shown below), which depicts a fairly typical sheet metal bent part: the outer contour is a 500×340 rectangle, with a diagonal reinforcing rib at each of the four corners, and two V-shaped bends forming reinforcing ribs in the center.

The overall height is 54, the sheet thickness is 3 mm, and the material is iron sheet.

Figure 1 Customer’s original drawing three views of 3mm iron plate bending parts (500×340×54)
Figure 1: Customer’s original drawing: three views of 3mm iron plate bending parts (500×340×54)

When many people see a drawing like this, their first instinct is to use SolidWorks’ sheet metal commands (base flange, edge flange, and bevel flange) to build it feature by feature.

But as soon as you try it yourself, you’ll discover that using a combination of base flanges and edge flanges to model this type of sheet metal part with beveled edges not only results in an extremely long feature tree, but also means that whenever you need to change the dimensions, you have to adjust nearly every flange feature—which is a real headache.

A Shift in Thinking: First, Break the Entire Part Down into 3 Pieces

Experience tells us: For parts that can be made using bending and welding, there’s no need to struggle with a single sheet of metal.

We can naturally break this part down into three sections based on the bending locations (as shown in the figure below):

The middle section, “Main Body 3,” connects the left and right halves;

One symmetrical “Side Panel 1” on the left and one “Side Panel 2” on the right, each featuring a reinforced structure with beveled edges.

Figure 2. The entire piece is disassembled into 3 bent parts ① Side plate 1 ② Side plate 2 ③ Main body 3
Figure 2. The entire piece is disassembled into 3 bent parts: ① Side plate 1 ② Side plate 2 ③ Main body 3

Once it’s disassembled, the problem becomes straightforward: there are three parts, each of which is a separate sheet metal component.

We just need to figure out how to draw the flat patterns for each part, and then cutting, bending, welding, assembly, and drafting will all fall into place naturally.

Step 1

First, extrude a “solid” to serve as the base for the sheet metal part.

The “Convert to Sheet Metal” command in SolidWorks requires a solid (or sheet metal part) as input, after which we use “edges” and “bend lines” to define the bend locations.

Therefore, we must first model this bent part as a regular solid.

Here’s how to do it: First, create a symmetrical cross-section on the front view reference plane (as shown in the figure below, with a total width of 340 and a 110-wide V-shaped bend contour in the middle), then use the “Extrude Boss” command to extrude it by 500 to obtain a symmetrical solid.

Figure 3. Symmetrical section drawn on the reference plane (critical dimension 110 340)
Figure 3. Symmetrical section drawn on the reference plane (critical dimension 110 340)
Figure 4. Click the Extrude Boss button to prepare to extrude it into a solid
Figure 4. Click the Extrude Boss button to prepare to extrude it into a solid

We set the extrusion length to 500, which is exactly equal to the total length of the customer’s original drawing.

After the extrusion is complete, we use the same method to draw a symmetrical cross-section on the other face and extrude it by 500 to obtain the final solid (as shown below).

Figure 5. Extrusion length 500, generating the first solid segment
Figure 5. Extrusion length 500, generating the first solid segment
Figure 6. Extrude another face to obtain the final solid object.
Figure 6. Extrude another face to obtain the final solid object.

Step 2

“Cut out” the sheet metal part we want from the solid.

The solid has been created, but we don’t need the entire piece—we only want a specific bent section.

In SolidWorks, you use the “Extrude Cut” command to remove the unwanted portions, leaving behind the base sheet metal part we need.

Take “Side Panel 2” as an example: We create a new sketch on a specific face of the solid, preparing to cut away regions 1 and 3 and retain only region 2 (as shown in the figure below, where the blue-highlighted face is the sketch reference plane).

Figure 7. Selecting a face as the sketch reference plane (highlighted in blue)
Figure 7. Selecting a face as the sketch reference plane (highlighted in blue)

There’s no need to redraw the sketch. Simply use the “Convert Entity References” feature to reference several edges from the entity into the current sketch.

This way, the sketch will naturally align with the entity, and there will be no misalignment.

Figure 8. The Convert Entity Reference command in the toolbar
Figure 8. The Convert Entity Reference command in the toolbar
Figure 9. Referencing entity edges to the current sketch
Figure 9. Referencing entity edges to the current sketch

The reference edge is broken at the bend location.

We use the “Extend” command to connect the broken segments, forming a closed contour (as shown below).

Figure 10. A closed sketch outline is obtained after extending and connecting
Figure 10. A closed sketch outline is obtained after extending and connecting
Figure 11. Click Stretch Cut to cut the solid using this contour
Figure 11. Click Stretch Cut to cut the solid using this contour
Figure 12. After the excision is completed what remains is the mother body of Side Plate 2
Figure 12. After the excision is completed, what remains is the mother body of Side Plate 2

Step 3

Convert the solid to a sheet metal part.

Now that the solid is positioned, it’s time for the core step of sheet metal modeling—click the “Convert to Sheet Metal” button (as shown below).

This command allows you to set key parameters such as sheet thickness, bend radius, bend lines, and reference planes.

Figure 13. The Convert to Sheet Metal button in the Sheet Metal toolbar
Figure 13. The Convert to Sheet Metal button in the Sheet Metal toolbar
Figure 14. Left hand Sheet Metal Parameters panel reeady to begin setting
Figure 14. Left-hand Sheet Metal Parameters panel ready to begin setting

Step 4

Set the sheet metal parameters (sheet thickness/radius/bend line / K-factor).

In the “Convert to Sheet Metal” Properties Manager that appears, set the following options in order:

“Fixed Solid Face”: Select the face that will remain stationary after bending (in this example, select the bottom face shown in the figure below).

Figure 15. Select Fixed Solid Face the side that remains stationary during bending
Figure 15. Select Fixed Solid Face: the side that remains stationary during bending

“Thickness”: Enter 3.00 mm, in accordance with the customer’s drawing specifications.

“Inner bend radius”: Set to 0.2 mm in this example.

Figure 16. Setting the plate thickness to 3mm and the inner corner radius to 0.2mm
Figure 16. Setting the plate thickness to 3mm and the inner corner radius to 0.2mm

Next, select the “bend line”—that is, the line that needs to be “flattened” when this sheet metal part is unfolded.

In this example, we need to unfold the V-shaped bend in the middle, so select the two bend lines marked in the figure below.

Figure 17. The positions of the two bend lines to be selected
Figure 17. The positions of the two bend lines to be selected
Figure 18. Selecting a specific bend line on the entity.
Figure 18. Selecting a specific bend line on the entity.

Finally, there’s the “K factor”—this parameter directly determines the accuracy of the unfolded length calculation.

We recommend not simply using the default value; instead, set it based on your factory’s bending experience:

For common 3mm steel plates, a value between 0.4 and 0.5 is typically used.

You can start by setting it based on experience, then calibrate it by actually bending one or two pieces.

Figure 19 Setting the K factor (values ​​based on our factory's bending experience)
Figure 19 Setting the K factor (values ​​based on our factory’s bending experience)
Figure 20. After setting all parameters, click OK
Figure 20. After setting all parameters, click OK

Step 5

Click “Unfold” to generate a flat pattern.

After converting to a sheet metal model, the model remains in a bent state.

Click the “Unfold” button on the toolbar to flatten the bends, resulting in a flat pattern that is ready for cutting.

Figure 21 Click the Expand button
Figure 21 Click the Expand button
Figure 22 Final plan view of Side Panel 2 (can be directly cut to size)
Figure 22 Final plan view of Side Panel 2 (can be directly cut to size)

Step 6

Follow the same procedure to create “Side Panel 1.”

Once you’ve gotten the hang of making the previous part, the rest is just a matter of repeating the process:

Save the complete solid from earlier as a new part file;

Use the same sequence of “Convert Solid Reference + Extend + Extrude Cut” to cut out “Side Panel 1”;

Then “Convert to Sheet Metal” and set the same parameters (3 mm / R0.2 / same K factor);

Click “Unfold” to obtain the flat pattern for “Side Panel 1.”

Conclusion

To sum up, splitting complex reinforced sheet metal components into multiple individual parts greatly simplifies modelling and flat pattern development in SolidWorks.

By building the base solid, trimming redundant geometry, converting solids into sheet metal bodies, configuring bending parameters including thickness, bend radius, and K-factor, and unfolding each segment one by one, we can reliably obtain accurate cutting layouts.

This “disassemble – unfold – reassemble” thinking avoids bloated feature trees and tedious dimension edits.

Mastering this method will help engineers efficiently handle comparable bent and welded sheet metal projects in daily design work.

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