Modeling Spot Welds
Introduction
The Spot Welds node in the Shell interface is intended for global analysis of structures connected with a large number of spot welds. The details of the spot weld as such is not modeled. An elastic connection is established between the two shell faces.
The connection is mesh independent, and the locations of the spot welds are specified using a list of coordinates. However, you cannot use arbitrarily large elements. The element size at the spot weld location should not be significantly larger that the diameter of the weld nugget.
Modeling Using the Spot Welds Node
The location of the welds is given in a table in the Nugget Location section. In most cases, you will import this table from an separate text file using Load from file ().
Nugget File Format
The format of the file is simple. Each weld is represented by a single line with 4 entries separated by white space:
<Nugget_number> <X_coordinate> <Y_coordinate> <Z_coordinate>
Any line that starts with a hash sign (#) is treated as comment and is ignored.
The exact location of the nugget does not have to be perfect. The given location is projected to the nearest point on the destination boundary. Thus, the nugget coordinates can, for example, represent an average location of the nugget (between the plates) or be placed on either plate.
Connected Location
The coupling is intended to operate between two adjacent physical surfaces, possibly at some small distance. That is, for each of the connected shells, it is either the top or the bottom surface that is connected. In most cases, the surfaces to be connected can be determined automatically. The algorithm measures the four possible distances between top and bottom sides of source and destination, and use the pair that has the smallest distance.
You can choose to manually specify which surfaces to connect. To do that, change Connected location from Automatic to Manual.
Nugget Stiffness
The elastic properties of the nugget is represented by an axial stiffness (kn) and a shear stiffness (ks). You can provide these values explicitly.
The default is to compute the stiffness using the properties of a thin layer. The thickness of the layer is a user input, named Cohesive thickness. The stiffness of the weld is inversely proportional to this value. Physically, the cohesive thickness can be seen as representing the part of the nugget that is located between the two plates. This is, however, not the full truth, since the local stress and strain field around a real spot weld is complex. Even an ideal weld, where there is no distance between the plates, will have some flexibility.
When computing the nugget stiffness, the elastic properties are taken from the destination boundary.
Mesh Size and Numerical Integration
The spot weld connection is mesh independent, in the sense that it is neither a node-to-node connection or a specific mesh element. Instead, a thin elastic layer is added over an area that approximates the size of the weld nugget.
Still, to achieve good accuracy the mesh must not be too coarse; the coupling uses a numerical integration on the destination boundary, and a large enough number of integration points are needed. A rule of thumb is that the element size (in terms of edge length) should be smaller than the nugget diameter.
More information about numerical integration can be found in the following blog post:
 www.comsol.com/blogs/introduction-to-numerical-integration-and-gauss-points
When a coarse mesh is used, you can improve the accuracy by increasing the number of integration points per elements. To do that, clear the User automatic quadrature settings checkbox in the Quadrature Settings section.
Figure 2-39 shows conceptually how two boundaries are connected by a spot weld.
Figure 2-39: Illustration of spot weld connection.
Below is a detailed explanation of the figure:
•
The yellow ball represents the nugget location on the destination boundary. It may have been placed there by projection.
•
The yellow cylinder represents the nugget diameter. It has the nugget location at its center.
•
The green mesh is located on the destination boundary.
•
The gray elements are the elements on the destination boundary that are involved in the connection. They have at least one integration point (Gauss point) inside the nugget diameter.
•
The black elements are the elements on the source boundary that are involved in the coupling.
•
The green arrows indicate how displacements are mapped from the source boundary to destination boundary.
•
Each arrow has its head located at an integration point on the destination boundary. The default integration scheme, shown here, uses 4x4 integration points per element.
You can check the interpretation of the connection by adding a Nugget Location plot from Result Templates. as shown in Figure 2-40. In this plot, each nugget is indicated using a red color. Also, each integration point that contributes to the nugget stiffness and force calculation is shown in blue.
Figure 2-40: Closeup in a Nugget Location Plot.
If you want to investigate the distribution of integration points using another integration scheme, you can modify the Gauss-point order setting in the Evaluation section in the settings for the Point 1 plot in the Nugget Location plot group.
Performance Considerations
The mapping between the connected boundaries can take a significant time if many boundaries are coupled, or there are many mesh elements. If this is a problem, there are three methods you can use improve the situation:
•
Split the selections into several Spot Welds nodes.
•
Set Connected location to Manual.
•
In the Advanced section in the settings for Spot Welds, change the Search method to Manual, and set a suitable Search distance.
Results
In many cases, you are only interested in the spot welds as a means of obtaining a proper global stiffness of a structure. You can also access the results in the individual welds.
From the Result Templates window, you can add:
•
A Spot Welds Forces plot group, to show the normal and shear forces at each weld, and a label showing the identity number of each weld. Normal forces are plotted as green arrows, and shear forces as blue arrows. To display the spot weld forces, these have to be evaluated first using the Spot Welds Normal Forces and the Spot Welds Shear Forces evaluation groups.
•
A Spot Welds Normal Forces evaluation group that contains a table of the location and the normal forces of all welds. Evaluate this table to display the forces in the Spot Welds Forces plot group.
•
A Spot Welds Shear Forces evaluation group that contains a table of the location and the shear forces of all welds. Evaluate this table to display the forces in the Spot Welds Forces plot group.
•
A Spot Welds Forces Magnitude evaluation group that contains a table of the normal and shear forces magnitude of all welds. In the table, select Show Row Numbers to display the number of each fastener.
Other results that are available are the bending and twisting moment in each spot weld, as well as the total force transferred by all spot welds in a Spot Welds node.