SOLIDWORKS Weldments from Profiles to Cut Lists - Part2

Welcome to the second part of the SolidWorks Weldments blog series! In this section we will look at creating:

  • Sketches for Weldments
  • Weldment Structural Members
  • Options for End Conditions

Where to start?

Either closed or open 2D Sketches can be used, it doesn't matter. SOLIDWORKS Weldments uses closed profile sketches to sweep along the sketch segments.


We will join a 3D Sketch to this skeleton. (3D Sketches are located on the Sketch drop down menu)


Now we will create a Structural Member based on these sketches. To access the Weldments tool bar right click the dark grey tabs below the Command Manager ribbon.


Once the Weldments tab is accessible you should be able to select the Structural Member button. A closer look at the Weldments toolbar:


You can select any size you want from the Standard menu. In this case I used a Square Tube. Click inside the Groups box to start your sketch selections.
The Groups box allows you to pick up sketch segments that belong to the same section of the Weldment. Here we are just picking the lines from the 2D sketch.


SolidWorksThere are many Settings to sort through. Here is a closer look.

Apply Corner Treatment allows us to specify a corner option for the whole Weldment.
These settings can be applied individually at each corner by right clicking the pink dot
as seen in the above image.

Merging allows you to make the selected segments all one body. This can affect your cut list, especially when your Structural Member is made up of several arc segments.

The G1 and G2 allow for weld gaps to be created between the Weldment sections.

Mirror does just what is says. You wouldn't notice much of a difference in this example as
the profile is that of a square tube.

Alignment, this allows us to change which axis of the sketch to align to an entity in the sketch.

Rotation angle of the profile can be set here.

Locate Profile, this button allows us to move to a different vertex or point inside of the profile
sketch. We will see this in the next few images.

This is an image of the default profile location.


After clicking the Locate Profile button we can choose any vertex or point in the sketch and the profile will move.
Now that we have the profile positioned, use the green check mark to accept the Structural Member.


Start a new Structural Member and pick the line segments of the 3D sketch. Use these settings for the End Condition and Gap.


Let's focus in on this corner to see the settings we have applied. Currently the profile is shifted, we will need to use the Locate Profile button
again to align the profile to the existing Weldment.


Here is what the alignment should be.


After confirming the Structural Member command you will notice that the tubes intersect. They will need to be trimmed.
This will be covered in the next section of the Weldment blog series article.

Please check back to the CATI Blog as the Dedicated Support Team will continue posting our series of articles that goes further into the details of SOLIDWORKS Weldments. All of these articles will be stored in the category of Daily Dose…..of SOLIDWORKS Support and links to each article with their release date are listed below:

Thank you for reading!!
John Van Engen
CATI Senior Technical Analyst

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