A common question that comes up in my training classes is : What should be examined – Nodal Stresses or Elemental Stresses?

When running a COSMOS analysis, the solver internally evaluates the stresses for each element in the model at specific locations inside the element (also called as Gaussian or Quadrature points). These points form the basis of numerical integration schemes used in Finite Element codes.

The number of points selected is determined by the type and quality of the element. The subsequent stresses obtained at the Gaussian points inside each element are extrapolated to the nodes of the element.

Now, let us consider multiple elements sharing a node. In such a case, what would be the stresses at the node, if the gaussian point inside each element contributes a stress value to that node?

* Nodal Values *are the averaged values of stresses at each node. The value shown at the node is the average of the stresses from the gaussian points of each element that it belongs to. In the adjoining figure, the central node would carry a stress that is an average of the 6 stresses coming from the 6 elements that it belongs to.

The alternative method of displaying stresses is called * Elemental Values*. In this method, each element individually looks at the stresses at its nodes from the Gaussian points. The stress at the element is the average of the stresses seen at its corresponding nodes.

**What stresses should one examine when taking a look at the stress plot?**

Since the approach to average stresses is different for the two methods, the maximum stresses in the stress plot will be different. In the above two examples, the maximum values from nodal and elemental stresses are 5 and 5.66 respectively.

The degree of difference in the values is a reflection of the coarseness of the mesh, and hence the convergence of stress results. If the values are very different, it is a reflection of the mesh being too coarse at the high stress location. Hence, the mesh needs to be refined at those locations using Local Mesh Control.

Comparing nodal stresses and elemental stresses is a way of understanding if the mesh is fine enough, and if the results have converged at the highest stress location in the geometry.

I got the idea for using Nodal and Elemental Stresses for convergence. Few suggest that 10% can be taken as criteria for convergence. but question is, which one to use? While designing we have to ensure a margin from failure point which in my case I am using say 10%. Now this additional 10% will make my margin 20% for say elemental stress and 10% margin for nodal stress. So my question is, which stress is better representation of actual stress. Elemental or nodal with which we can decide failure?

Hi Kuldeep,

In practice, regardless of whether you use either averaging schemes, as long as you progressively refine the mesh in the areas of concern until the energy norm error drops below 10%, you should be good.

Actually, the stress error estimation is based on the principle of the continuity of stress. The resulting stress distribution of a finite element analysis is generally discontinuous. The nodal stresses of each element are averaged to smooth the discontinuity in the element stresses, and is often used as the baseline. The stress error in each element is defined as the difference between the element stress and the average of the nodal stresses corrected using the form functions. This error is used to calculate the energy norm error for each element. SOLIDWORKS Simulation allows the user to plot a contour of the percentage of the elemental energy norm error relative to the average elemental energy (see the plot called ERR when you create a stress plot on elemental values).

If this value drops below 10%, the mesh is generally considered as an adequate representation of the model, and hence the results should be in line with expectations.

you suggest to ensure the average elemental energy ( plot called ERR ) is less than 10%. Does this means the ERR plot is less than 10, or less than 0.10? thank you.