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Using a solid model as reference geometry for creating a SOLIDWORKS Weldment Sketch

Article by Mehdi Rezaei, CSWE created/updated January 31, 2017

There are a lot of techniques for creating a SOLIDWORKS Weldment Sketch on the web and in the help file. Despite that fact we are often asked what is the easiest and most effective method of creating a Weldment Sketch. In this blog article, I will show you a quick method of using a solid model as reference geometry when creating your 3D Sketch.

The following image depicts a 3D solid model created by a boss extrude with a draft angle. Having the basic knowledge of SOLIDWORKS part modeling helps to quickly create the required shapes. This solid body represents the shape of my required weldment.

Create a Solid Model

Convert Edges to a 3D Sketch

Now that we have a solid body created, start a new 3D sketch and then run Convert Entities to select and convert all the edges of the solid model into the active 3D sketch. In this case, every single edge has to be selected one by one to be added to the selection box of the Convert Entities command. At this stage, extra attention must be paid to make sure none of the edges are left out.

Quicker Way of Selecting Edges

There is a much quicker and more reliable method to select edges. Once a 3D sketch is active, click on one edge and then hit Ctrl+A on the keyboard. This will pick all the edges of the model and have them selected. At this stage if Convert Entities command is selected, all those edges will be converted to the active sketch. Now we can use this 3D Sketch for Weldment modeling, add profiles, etc.

Convert Entities

Hide the reference Solid Body

Once the 3D sketch is created, the solid body can be hidden from the feature tree as shown in the following image. Now the 3D sketch is ready to be used for the weldment modeling. The advantage of this method is that the angle of each line follows the draft angle of the associated face and as a result the orientation of the lines have to be correct. Therefore, extra reference planes would not be needed.

SOLIDWORKS Weldment Sketch created

Hide Solid Body

Modifying the Final Weldment Model

Weldment models can sometimes be tricky. Although the dimensions and relations work fine at first, when making a quick modification can sometimes cause the 3D sketch to become corrupted. Using a 3D solid model as reference geometry makes it easy and more reliable to make design changes. Simply modify the reference model dimension or shape and the changes will be reflected in your weldment design.

Dimension Adjustment

Learn more about Weldments

Attend our SOLIDWORKS Weldments course either online or in a Canadian city near you.

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Mehdi Rezaei, CSWE

Mehdi is a Certified SOLIDWORKS Expert (CSWE) and works near Vancouver, British Columbia, Canada

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