SOLIDWORKS Weldment Sketch From Solid Model Tutorial

Article by Zach Brown on Nov 21, 2022

While many users leverage weldments inside of SOLIDWORKS, one of the main challenges is the creation of 3D sketches needed for the layout of structural members. In this tutorial, learn how to use a solid model in SOLIDWORKS to generate and parametrically drive 3D sketches, foregoing the hassle of creating them manually.

Traditional SOLIDWORKS Weldment Setup 

Typically, when creating weldments in SOLIDWORKS, there can be multiple 3D sketches needed to lay out the paths for structural members. It can be challenging to maintain design intent when working with multiple 3D sketches that have relationships to each other.

SOLIDWORKS Weldment Setup

The usual process is, once the layout sketch is complete, to add a structural member and create groups by selecting individual sketch entities.

Structural Member Options in SOLIDWORKS

Solid Model Approach

Now that we have seen the traditional method of creating weldment sketches, we will show how to create them using a solid model. Here we have a solid model representation of the 3D sketch layout. This was created from three 2D sketches on different parallel planes. Sketches were then lofted together.

SOLIDWORKS Weldment Sketch from Solid Model Tutorial

The edges of the solid represent the paths for our structural members, so we will convert them into a single 3D Sketch. 

Start a 3D Sketch by going to Sketch Toolbar > Sketch Flyout Menu > click 3D Sketch.

3D Sketch Option in SOLIDWORKS From Sketch Toolbar

Since we will need to select all the edges of the solid, turn on the Selection Filter and enable the Edge Filter.

Hit F5 on the keyboard to turn on the Selection Filter Toolbar. Click Edge Filter.

SOLIDWORKS Edge Filter Selection from Filter Toolbar

Now we need to select all edges. Since we enabled the edge selection filter, we can perform a Select All to capture all the edges simultaneously via Standard Toolbar > Select Flyout Menu > Select All.

Select All Edges in SOLIDWORKS

SOLIDWORKS Select All Edges Example

Now that all the edges are selected, the next step is to convert them to sketch entities. We will do this with a tool called Convert Entities.

Sketch Toolbar > click Convert Entities.

Convert Entities in SOLIDWORKS Sketch Toolbar

Once we have converted the edges, the result is a single 3D sketch parametrically driven by the edges of the solid model. 

Converted Edges in SOLIDWORKS

The next step is to add a structural member and select the sketch entities as normal for a weldment. For this example, I have created a base bottom sketch with dimensions to help with creating the solid model. Dimensions can be changed, and the weldment will update accordingly.

SOLIDWORKS Weldment Frame from SOLIDWORKS Model Example

Weldment Frame from Solid Model in SOLIDWORKS

As you can see, the solid model approach to weldment sketches can save time and help with maintaining design intent. I hope you found this tutorial helpful. Check out more SOLIDWORKS tips and tricks below.

GoEngineer YouTube Video SOLIDWORKS - Weldment Sketch From Solid Model Want to learn more? Check out this YouTube video for a demonstration of these tips, tricks, and best practices. 

SOLIDWORKS Weldment Training

Learn to build stand-alone sheet metal parts and create standard structural members by enrolling in professional SOLIDWORKS Weldment training with GoEngineer. Learn more below. 

Take a SOLIDWORKS Weldments Training Course from GoEngineer

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About Zach Brown

Zach Brown is a certified SOLIDWORKS Expert and a Technical Support Engineer. Prior to working at GoEngineer, he spent 15 years as a mechanical designer, CAD support tech, and instructor using SOLIDWORKS. His hobbies include playing guitar, riding motorcycles, and skiing.

View all posts by Zach Brown