- Introduction:
Abaqus offers a range of methods to help finite element analysts build confidence in his/her results. This blog by Nicholas Hopwood, a member of Simulia UK technical team provides a small insight into a few of these methods to identify potential areas of obscure results caused by discontinuities in a model.
-Mesh Density:
Firstly and most importantly for accurate resolution of results is to have a sufficient regular mesh and correct element selection, for the type of analysis being performed.
If a mesh is too coarse then the inherent element approximations will not allow an accuarate solution to be obtained. Alternatively, if the mesh is too fine the cost of the analysis can be out of proportion to the results obtained.
To define an appropriate mesh it can be useful to consider the stress distribution that is expected. In regions of high stress/strain gradients and change rates the mesh should be finer and in regions of constant stress/strain a coarser mesh can be used. [1]
How do I know if my mesh density/refinement is sufficient?
An example mesh convergence study has been performed in the Getting Started with Abaqus Manual: 4.4 Mesh Convergence. It describes a potential methodology used to ensure a converged mesh has been reached with reasonable results to simulation runtime ratio. Basically this means refining the density of the mesh and looking at the effect it has on the results at regions of interest in a model.
What can cause inaccuracies in my mesh/results?
High rates of change of stress will occur where there is any form of discontinuity; generally in geometry, or in the loading, or in the material properties. Generally a finer mesh is required in such regions. The equations of elasticity are such that any form of discontinuity only produces local disturbances which die away with distance (St Venant’s Principle). This effect means that for accurate results the finer mesh at the region of discontinuity can be graduated to a coarser mesh with distance from the area of discontinuity. [2]
To estimate these die away distances the user must have an understanding of the way the structure behaves. It is not possible to give a rule of thumb because different geometries with different materials, loadings, etc have different die away distances.
So what methods can be used to highlight the regions of discontinuities in my mesh/results?
1) Discontinuities result plot in Abaqus (Preferred Approach):
In Abaqus Visualisation Module: Result -> Option -> Discontinuities Contour Plot.
The discontinuities plot displays the differences in field output values between adjacent elements. The Abaqus/CAE User’s Manual: 42.5.2 states:
“Discontinuities: 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 you select. 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.”
Further discussion in displaying the Discontinuity plots are found in the Abaqus/CAE User’s Manual 42.5.5: Displaying field output values or discontinuities.
Fig 1: Comparison of mesh refinement on pressure loaded surface for Mises Stress plot. Coarse Mesh -> Wide spread discontinuities, Finer mesh -> Smaller localised discontinuities.
2) Output variable SJP:
So what are Stress/Strain Jumps?
Stress and strain results are derived from the displacements and so are not conforming, leading to the accuracy varying more widely over each element. Along common sides or edges it will be seen that they differ between meeting elements. In the present context stresses hold similar conclusions as strains. All the stresses components calculated at a common node will be seen to differ when calculated at each of the adjacent elements, producing a lack of equilibrium known as a stress jump. As the mesh is refined the magnitude of this jump should drop. It is important to note that for any point the error in the stress component with the largest magnitude affects the other stress component errors by a similar magnitude due to a Poisson’s ratio effect. Thus the smaller components absorb this error and dominate their own errors. This reduces the accuracy of the lesser magnitude components. Only the stress component with the largest magnitude has a realistic error due to the state of convergence of the analysis. [3]
What is, and what does Abaqus Output SJP (Strain Jump at Nodes) show?
A nodal error estimate to show 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 if a mesh is fine enough such that for any given node all the elements attached to it have nearly the same stress/strain. For coarse meshes in areas of rapidly changing stress/strain, adjacent elements sharing one or more of the same nodes may calculate dramatically different stress or 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. This output variable is available only in Abaqus/Standard as output to the. dat and the .fil file. [4]
What is averaging and what are the different options associated with it?
The results for an element are stored at the integration points. For visualization purposes in Abaqus/CAE these results are extrapolated to the nodes and averaged. The following Simulia visual tip attempts to give some more information about the averaging schemes in Abaqus.
Answer Title: SIMULIA Visual Tips: Averaging results across feature edges in Abaqus/CAE and Abaqus/Viewer
Answer Link: http://simulia.custhelp.com/cgi-bin/abaqus.cfg/php/enduser/std_adp.php?p_faqid=3593
[1] – NAFEMS: A Finite Element Primer, Pg 94, 4th Reprint 2003.
[2] – NAFEMS: A Finite Element Primer, Pg 94, 4th Reprint 2003.
[3] – NAFEMS: How to use Elements Effectively, Pg 99, 2003.
[4] – NAFEMS: A Designer’s Guide to Simulation with Finite Element Analysis, Pg 55, 2008.
