Home » How to add weldments in SolidWorks?

The weldment feature in SolidWorks is a powerful tool. It can be used to insert individual beams or to create and entire frame structure for fabrication. There are two methods for inserting a structural member into an assembly, these will be described in detail. There are also various methods, to create the geometry for placement of members, when creating a frame.

How they Work


SolidWorks has structural profiles (weldment profiles) saved as library features. When a structural beam is selected for insertion, SolidWorks sweeps the profile to the length of the selected reference. When two segments are connected in a sketch, the result is two separate weldment bodies.

Weldment Template Creation

Open an existing part template and select the weldment tab of the CommandManager. Click on the weldment button to mark the part as a weldment part. Save the file as a part template (.prtdot). Use this template for creating weldment parts.

Step 1 – Creating Beam Geometry

2D Sketch Methods

Skeleton Sketch

Begin with a 2D sketch on the right plane. Sketch the structure of the sides of the frame using  lines.  Dimension the sketch so that it is fully defined.  Once complete, offset two planes at either side of the right plane.  Set both offsets as half of the width of the desired frame. Create a sketch on each plane and use convert entities to reference the lines created in the first sketch.  The final step is to interconnect the two sides with cross members. Create a 3D sketch and connect the two sides using lines.

Edit dimensions for the sides using the initial sketch. The width of the frame can be edited by moving the planes.

Reference Grid

This method is similar to the 2D skeleton sketch, instead of creating the offset planes, use insert grid. Select a plane for the initial sketch, then select “Insert” – “Reference Geometry” – “Grid System”. This will launch a sketch editor relating to the grid system option.  Draw the necessary 2D geometry  as shown above. Upon exiting the sketch, the GridSystem options will appear. For the frame shown above set the values of instances to 2 and default height to 1200mm. The image below is to indicate that multiple levels can be created at once, and that the height for each level can be manually altered.

The grid system will automatically interconnect the sketches for placement of cross beams. If the 3D sketch does not appear, expand the grid system feature in the DesignTree and set it to visible.

Surface Extrude

Similar to the previous methods, begin by creating the 2D sketch of the frame structure. Once complete, use extrude surface from the surface tab of the CommandManager. The final step is to create a 3D sketch, use convert entities to reference the edges from the extruded surface.

Surfaces do not add mass to the model, there is no need to delete the surface extrude after creating the 3D sketch.

3D Sketch Method

The process is the same as described above, this time use a 3D sketch to create the entire frame. To constrain entities in 3D sketches there are various options. One vertical beam has been constrained to 1750mm from the corner post, on the opposite side the line is constrained using a construction line along the X-axis. The other two lines  (3250mm) have been constrained on a plane. This has been done to illustrate how quickly 3D sketches can become complex for editing.

It should also be noted that placement of dimensions is dependent on the entities selected. One 1750mm dimension was placed by selecting the lines, the other by selecting the points.

Step 2 – Placement of Structural Members

Into Parts

A single beam can be placed, to do this first create a 2D sketch with a line of the desired length. The next step is to select structural member from the CommandManager. In the options select the desired structural member profile and size, then select the line that was sketched.

Inserting Members

Now that the frame has been sketched, members can be added. Click on the Structural Member on the Weldments tab of the CommandManager.  Use the following settings:

  1. Standard – ISO.
  2. Type – square tube.
  3. Size – 80 x 80 x 5.
  4. Groups – 3 groups will be required. Group 1 will be the vertical corner members. Create a new group and select the long horizontal lines for placement of beams. The third group is for the short horizontal members.

SolidWorks defines two rules for which members can be part of a single group.  The segments must either be connected end to end, or they must be parallel otherwise. Groups are used to automatically apply the correct end treatments to the beams. The trim operations applied follow a hierarchy, group 3 members are trimmed to the faces of connections to either group 1 or group 2 members. Similarly, group 2 are only trimmed to the connecting faces of group 1 members. The standard, type and size cannot change between groups.

Depending on the initial 2D sketch, trim/extend operations may be required to extend the vertical corner posts. Select trim/extend from the CommandManager.  Select all of the corner posts, use the bottom face of one of the horizontal members at the bottom of the frame as the trimming boundary. Do the same for the corner posts, this time select the top face of a horizontal beam at the top of the frame.

Tip: If the beam type and size are known, offset the lines in the 2D sketch to avoid the trim/extend operations.

Select the structural member button again, to add other member types or sizes. Use angle and the locate profile button to correct the orientation of the beams.

Into Assemblies

Insert weldments, as individual beams or entire frames, the same way a normal part is added.  Alternatively, beams can be inserted using the SolidWorks toolbox.

Some standards of the SolidWorks toolbox contain structural members that can be inserted into assemblies. Individual beams can be added to assemblies through drag and drop from the Task Pane. To do this, use the following instructions:

  1. Select Design Library from the Task Pane.
  2. Navigate through “BSI” – “Structural Member” – “Steel”, drag and drop the desired member into the assembly.
  3. Select the size from the available configurations.
  4. Input a length for the beam.

Frames can be create directly in an assembly, however they would take longer to create. The trim features of weldments allows for easy application of end treatments to beams. Creating the frames, in an assembly, would require these end treatments to be sketched manually.