# News / Blog

## Has my mesh converged?

**Has my mesh converged?**

Finite Element Method as we know is a numerical technique finding approximate solution for structural problems. When solving a finite element problem, how do we ensure that the solution we obtained is accurate? We have quite often heard the word ‘convergence’ in a non-linear static FEA. Convergence in a non-linear static analysis implies accuracy of solution based on convergence of finite element mesh as well as convergence of non-linear solution procedure. As discussed before, the approximation in a FEA comes from mesh as well. The geometry is discretized into finite number of small elements. Increasing the number of elements in the model will cause the solution to approach the analytical solution. At some point further mesh refinement yields little or no change in solution, and the mesh is assumed to have converged. Of course there are some exceptions to this such as fracture and damage class of problems. In this article let us take a look at what do we mean by mesh convergence and how do we ensure the finite element mesh is converged in Abaqus.

Abaqus offers few convenient ways to evaluate mesh convergence. Abaqus/Viewer, the visualization module of Abaqus/CAE offers some contour options to check for mesh convergence. One of the contour plot options is **Quilt** contour. Quilt contour plot is an effective means of displaying results on an element-by-element basis. The values are computed for each element face individually with no averaging across element boundaries. Hence it shows the difference in values across individual elements against neighboring elements thereby giving a reasonable idea about mesh convergence. Quilt plot options are available only for element based outputs.

The other contour options that can be used to study mesh convergence is **Discontinuity** plot. Discontinuities are the differences in field output values between adjacent elements. For the display of discontinuities, the calculated invariants or components at nodes common to two or more elements are compared to determine the greatest difference, depending on the compatibility of contributing result regions and on options selected. Nodes associated with only one element and nodes receiving equivalent values from all contributing elements will show a value of zero in a plot of discontinuities. The discontinuity plot gives more visibility on the mesh convergence by doing the above.

The one other form of output that could be used for mesh convergence study is **Strain Jump at Nodes (SJP). **This output is only available in Abaqus/Standard and only available for printing it to a DAT file or FIL file. It shows a nodal error estimate of the strain jump between nodes which can be used as a measure of how rapidly the strain is changing at each node in the model. Ideally a mesh is fine enough such that for any given node, all the elements attached to it have nearly the same strain. For coarse meshes in areas of rapidly changing strain, adjacent elements sharing one or more of the same nodes may calculate dramatically different strain values. When the adjacent nodes have the same strain values the error is zero and when the nodes have different values the error is positive, naturally the closer the error to zero the higher confidence in results.

To conclude, **Quilt plots**, **Discontinuity plots** and **SJP (strain jump at nodes)** output variables are effective tools to quickly check mesh convergence and have confidence on the analysis results in the context of the finite element mesh.