Different Ways to Bend a Part in SolidWorks

While you may be accustomed to one specific bending technique in SolidWorks, exploring alternative methods can significantly enhance your design flexibility. Understanding the various ways to bend a part in SolidWorks is essential for tackling diverse design challenges, from simple enclosures to complex assemblies. This knowledge allows you to select the most appropriate approach based on the part’s geometry, manufacturing requirements, and material properties.

Basic Bend Types in SolidWorks

Mastering the fundamental bend types is key to effectively bending parts in SolidWorks sheet metal designs. When converting a solid body to a sheet metal part using tools like Insert Bends or Convert to Sheet Metal, you can apply three primary bend types: sharp bends, round bends, and flat bends. Each type suits specific geometries and helps ensure accurate flat patterns for manufacturing.

Sharp Bends

Sharp bends are ideal for models with sharp corners and uniform thickness throughout. They create precise, angular transitions without radii, commonly used in brackets or frames where tight corners are required. For example, in structural components like metal shelves, sharp bends provide clean edges that align well with assembly constraints.

Round Bends

Round bends apply to models featuring filleted or rounded edges with consistent thickness. These bends incorporate a radius, making them suitable for parts that need smoother transitions to reduce stress concentrations. Conical and cylindrical faces can also generate round bends, which are often seen in ductwork or piping enclosures. According to SolidWorks documentation, round bends help maintain material integrity during forming processes.

Flat Bends

Flat bends are created by drawing bend lines directly on the flattened sheet metal part. These lines appear in the Flat-Sketch under Process-Bends in the FeatureManager design tree and are visible across the model. This type is useful for custom bends that don’t follow standard edges, such as in irregular panels or artistic metalwork.

Using the Bends PropertyManager

The Bends PropertyManager is essential for converting shelled parts into sheet metal and applying bends accurately in SolidWorks. It provides control over parameters like radius, allowance, and relief, ensuring the design aligns with manufacturing standards.

To convert a part to sheet metal using the Bends PropertyManager:

1. Click Insert Bends from the Sheet Metal toolbar, or go to Insert > Sheet Metal > Bends.
2. Under Sheet Metal Parameters, select Use material sheet metal parameters to apply settings from the chosen material.
3. Under Bend Parameters:
   • Select Override default settings to modify the bend radius or thickness from the default sheet metal feature.
   • Choose a Fixed Face or Edge.
   • If the part lacks a planar face, select a linear edge instead.

3. • Specify the Bend Radius.
   • Select Ignore beveled faces to prevent chamfers from converting into sheet metal bends.
4. Under Bend Allowance, choose from Bend Table, K-Factor, Bend Allowance, Bend Deduction, or Bend Calculation.
5. If selecting K-Factor, Bend Allowance, or Bend Deduction, enter the appropriate value.
6. Enable Auto Relief and select the relief type (e.g., Rectangular or Obround), providing a Relief Ratio if needed.
7. Under Rip Parameters, select an edge and click Change Direction to adjust the rip direction. Enter a value in the Rip Gap box for the gap distance.
8. Click OK to apply the changes.

This process is particularly useful for imported models or solids created without initial sheet metal intent, allowing seamless integration into fabrication workflows.

Sketched Bends in SolidWorks

Sketched bends allow you to add custom bend lines to a flat face of a sheet metal part, enabling precise control over bend geometry relative to other features. This method is versatile for non-standard designs where bends must align with specific sketches or edges.

Sketch on sheet metal face and Sketched bend applied.

Key details for creating a sketched bend feature include:

• The sketch must contain only lines, with the option to include multiple lines per sketch.
• The bend line does not need to match the exact length of the faces being bent, offering flexibility in design.
• Sketched bends can be applied to non-planar flat faces, expanding their utility in complex parts.

Often paired with tab features, sketched bends are commonly used to create tabs or flanges that require unique orientations, such as in electronic enclosures or custom brackets.

The No Bends Option in SolidWorks

The No Bends tool temporarily removes all bends from a sheet metal part, allowing you to add features like walls or cuts in the flat state. This is available only for parts with Flatten-Bends and Process-Bends features, enhancing efficiency in editing.

Rolling Back All Bends

To remove all bends: Click No Bends on the Sheet Metal toolbar to roll back to Sheet-Metal. The bend allowance and radius are preserved, but the part remains unflattened, ready for modifications.

Restoring All Bends

To restore the bends, simply click No Bends again on the Sheet Metal toolbar.

This feature streamlines workflows, especially when integrating additional sheet metal tools without permanent alterations.

Changing the Bend Direction of a Sheet Metal Part

The bend direction in SolidWorks sheet metal parts is determined by the fixed face specified in the model. Adjusting this can flip the orientation, which is crucial for matching design intent or manufacturing preferences.

When editing the Flat Pattern feature in the Flat-Pattern folder, the current fixed face is highlighted.

To change the direction: Edit the Flat-Pattern feature and select a face on the opposite side of the material.

Select a new fixed face, and the bend direction in the sketch and drawing will update accordingly. This adjustment is vital for ensuring the part unfolds correctly for laser cutting or punching.

Unfold and Fold Features in SolidWorks

The Unfold and Fold tools enable selective flattening and bending of one or more bends in a sheet metal part, optimizing performance by focusing only on necessary areas. This is particularly beneficial for adding cuts across bends without affecting the entire model.

For instance, to add a cut over a bend: First, insert an Unfold feature to flatten the specific bend. Then, apply the cut. Finally, use a Fold feature to restore the bend.

To add a Fold feature:

1. Click Fold on the Sheet Metal toolbar, or go to Insert > Sheet Metal > Fold.
2. Select a Fixed face in the graphics area that remains stationary, such as a planar face or linear edge.

3. Choose one or more bends to fold, or select Collect All Bends for all suitable bends in the part.

4. Click OK to fold the selected bends.

These tools improve design efficiency, especially in iterative processes where features need to span bent regions.

Advanced Bending Methods: Lofted Bends

Beyond basic and sketched bends, SolidWorks offers Lofted Bends for creating transitional sheet metal parts between two profiles. This method is ideal for conical or tapered shapes, such as hoppers or funnels. You define two open sketches as profiles, and SolidWorks generates the bent geometry with options for bent or formed manufacturing methods. Recent versions, like SolidWorks 2025, enhance this with improved flat pattern accuracy.

Conclusion

Exploring the different ways to bend a part in SolidWorks—from basic types and sketched bends to advanced features like lofted bends—equips you with versatile skills for sheet metal design. Selecting the right bending method based on the situation can streamline your workflow, improve manufacturability, and reduce errors. With ongoing updates, such as the new bend notches in SolidWorks 2025 for better press brake alignment, staying informed ensures your designs remain cutting-edge.