In this tutorial, you will learn a practical method to connect rectangular tubes in SolidWorks. The workflow includes using weldments, cut-extrude, mirror features, fillets, and converting to sheet metal for bend operations.↳
Downloads
👉 Download the SolidWorks Part File (.SLDPRT) 👉 Download the STEP File (.STEP)↳
Skills You Will Practice
Using Weldments to create rectangular tubes↳
Applying Cut-Extrude on selected bodies↳
Using Mirror and Fillet features↳
Converting to Sheet Metal and applying Sketched Bends↳
Step-by-Step Instructions
Sketch on the Front Plane Draw a straight line as the path.
Weldments – Structural Member Choose a rectangular tube:
30 × 20 × 1.5. Alignment: rotate 90° or align with the vertical axis.↳Weldments – Add Another Tube Insert the horizontal tube.↳
Sketch on the Front Face of the Vertical Tube Draw a rectangle.↳
Cut-Extrude Depth:
5 mm.
Feature scope: only the vertical tube.↳Mirror Mirror the cut-extrude feature.↳
Fillet Radius:
2 mm.Sketch on the Front Face of the Horizontal Tube Draw a rectangle, then apply Offset Entities:
0.2 mm.↳Cut-Extrude End condition: Through All.↳
Convert to Sheet Metal Select one fixed face. Bend edges: collect all bend lines.↳
Sketched Bend
Sketch plane: inner face of the vertical tube.↳
Use Convert Entities to reference edges.↳
Fixed face: the face below the straight line.↳
Bend position: Bend Outside.↳
Bend radius:
0.2 mm.
Repeat on the Opposite Side Apply the same sketched bend on the other side.↳
✅ The connection of rectangular tubes is now complete.↳
Tips
💡 Use Feature Scope carefully to avoid cutting unintended parts. 💡 Sketched Bend is useful when you want more control over sheet metal deformation.↳
Related Tutorials
Beginner’s Guide: Designing a Plastic Box with Curved Surfaces in SolidWorks
0 Comments