Mesh Convergence Study Using ANSYS Nivrutti Garud, Engineer, Satyam Engineering Services Ltd. Secunderabad. E-mail:
[email protected]
Abstract: A finite element analysis for stress and displacement analysis is commonly used in the mechanical industry. The accuracy of the analysis results depends on the number of elements used for the FE analysis. The FE solution approaches to analytical (Exact) solution when number of element (Nodes) increases in the model. The accuracy of the finite element analysis solution for a given problem and mesh density can be measured in terms of descretization error. In this paper different methods to find out the mesh descretization error are discussed. The mesh convergence is studied for different element types and by varying the mesh density. ANSYS commercially available analysis package was used for the analysis.
Introduction: Displacement results are the primary results of a finite element analysis and other results are derived from the displacements. Displacement results are less sensitive to the number of elements or nodes in the model, but stress results vary much with increasing mesh density till the convergence is achieved. So it is very important to validate the stress results before concluding the analysis. A finite element element analysis requires requires the idealization idealization of an actual actual physical problem problem in to a mathematical model and then the finite element solution of that model. The solution should converge (when the number of elements increased in the model) to the analytical (Exact) solution of the differential equations that govern the response of the mathematical model [1]. Finite element solution approaches to analytical (Exact) solution when number of elements (Nodes) increases in the model. In linear elastic analysis there is a unique exact solution to the mathematical model (i.e. for given stress analysis problem). It is also important to note that convergence convergence is directly related to the load and constraints applied to specific run. Hence the mesh which is converged for particular loading and constraints may not converge to different loads and constraints.
Elements must be complete and the element and mesh must be compatible to insure the convergence for a given finite element mesh. The requirement of completeness of an element means that the displacement functions of the element must be able to represent the rigid body displacements and the constant strain rates [1]. The requirement of compatibility means that the displacements within the element and across the element boundaries must be continuous. Physically comparability insures that no gaps occur between elements when the assemblage is loaded [1]. Error Estimation: For mesh convergence to the exact results the elements must be complete and compatible. Using compatible elements mean that in the finite element problems the displacements and their derivatives are continuous across element boundaries. And the elemental stresses are calculated using derivatives of the displacements and must be continuous across the element boundaries. But the stresses obtained at an element edge (or face), when calculated in adjacent elements may differ substantially if a course finite element mesh is used [1]. This stress difference across element boundary decrease as the finite element mesh is refined. The stress jumps or stress difference across the element boundaries of the body are of course a consequence of the fact that stress equilibrium is not accurately satisfied unless a very fine mesh is used. Thus this stress jumps or stress gradient across element boundaries can be used as the measure of descretization error for a given mesh [1,2,3].
Methods of Error estimation: 1) Using Elemental Stresses: The discontinuity of stress across the element boundaries can be used for the error estimation. In order to establish a measure of stress difference across the elements it can be compared with the absolute maximum stress value that occurs anywhere in the model [3]. The error can be estimated using following formula [2].
Error = ((Si(max)-SJ(min))/Smodelmax)*100 Where Si(max) -is maximum elemental stress at element I S(min) -is minimum elemental stress at element j (Adjacent element to element i) Smodelmax -is maximum elemental stress in the model. Following example gives the error estimation for given four elements. Element i is the element for which the stress is maximum and element j is element for which stress is minimum.
Error = ((Si-Sj)/Si)*100
Element i
Element j
Figure 1: Element stress plot.
2) Using Nodal stresses: Similarly nodal stress can be used to find out the error in mesh convergence.
Error = ((Siu-Sia)/Smodelmax)*100 Siu -is maximum unaveraged stress (Elemental stress) at node i. Sia -is average nodal stress at node i. Smodelmax -is maximum averaged stress in the model. Analysis and results: General plane stress problem (Plate with hole) was considered for this study. The finite element model was modeled using quarter symmetry. Plane stress four noded element (Plane 42), ten noded tetrahedron element (Solid 92) and eight noded hexahedral element (Solid 45) were used to mesh the model and separate error estimation study was carried out. The element density was increased uniformly throughout the volume to study the effect of descretization. ANSYS V5.6.2 is used as pre and post processor. Steel material properties, Young’s Modulus 2.1e5 MPa and Poisons ratio 0.3 was used in the analysis.
Stress in X-direction (longitudinal stress) Sx is used for error estimation. The plate dimensions (in mm) are shown in Figure 2 below. Thickness of plate is taken as 10mm. Symmetric boundary conditions were applied at cut boundaries and force of 10000N was applied over the end as shown in the Figure 2.
80
40
20
10000N on this face.
Symmetric Boundary conditions on these faces.
Figure 2: Geometry and Boundary Conditions for the analysis.
Observation 1: The averaged nodal stress (using PLNSOL command in ANSYS) and unaveraged nodal stress (using PLESOL command in ANSYS) contours are given in Figure 3 and Figure 4 respectively. It can be seen that the maximum averaged nodal stress (using PLNSOL command) and maximum unaveraged stress (using PLESOL command) are not at the same node location. These stress values are at different node locations and hence can not be used directly for error estimation. In the present work the averaged and unaveraged stress at the same node location was considered for the error estimation.
Figure 3. Stress plot-using PLNSOL.
Figure 4: Stress plot using PLESOL.
Observation 2: If the maximum stress occurs at a corner node, and this node belongs to only one element, then the averaged and unaveraged stress at that node will remain same. In this case the error will be zero percent even if the mesh is course mesh. Following Figure 5 and Figure 6 gives the stress plots for problem where maximum stress occurs at the corner node belonging to one element.
Figure 5: Stress plot-using PLNSOL.
Figure 6: Stress plot-using PLESOL.
Also the averaging is generally done considering only the selected elements while plotting the stress contour. In this case actual averaged stress considering all the elements attached to that node may vary with the averaged stress when only few elements attached to that node are selected. Following tables gives the error in the region of maximum stress (at the element or node where the stress is maximum in the model). The error calculated using the two methods is compared with the strain energy error in the model, calculated using ANSYS. Result Table 1. Element type: PLANE 42 No. of Nodal Error Error strain nodes solution: (Elemental (Nodal energy Stress stress stress error (MPa) method) method) 49 93.65 49.78 1.09 14.476 83 101.29 41.93 1.19 13.358 101 104.89 32.78 0.01 11.691 146 106.95 27.51 0.09 8.88 251 108.65 20.80 0.02 8.94 491 109.21 15.37 0.00 6.03 1172 109.53 10.08 0.00 3.96 1342 108.92 7.65 0.00 3.51 Result Table 2. Element type: SOLID 45 No. of Nodal Error Error Strain nodes solution: (Elemental (Nodal energy Stress stress stress error (MPa) method) method) 196 107.16 40.48 0.00 10.43 210 104.44 38.50 2.33 10.43 456 111.28 31.19 1.33 11.58 950 112.24 29.05 0.04 7.49 3234 112.88 17.32 0.00 5.16 4799 113.18 17.25 0.00 4.86 Result Table 3. Element type: SOLID 92 No. of Nodal Error Error Strain nodes solution: (Elemental (Nodal energy Stress stress stress error (MPa) method) method) 3198 111.28 42.09 6.48 6.09 3689 110.84 31.68 4.13 5.09 4074 111.74 28.82 2.24 2.00 4151 112.04 18.65 0.97 1.46 9521 112.34 17.76 0.73 0.77 10527 112.24 17.76 0.43 0.56
From Result table 2, it can be seen that the error is zero calculated by nodal stress method for 196 nodes in the model (column 1). It is because of the stress is maximum at the node belonging one element (not shared by two or more elements; see observation 2). Conclusions: 1. Error using elemental stress gradient is more accurate method as the element results are absolute results (No averaging is done). Also comparing this method with nodal stress method this method is error free method and gives fairly good error estimation. This method is also suggested in literature (Books) very commonly. 2. Error using nodal stress has some disadvantages and gives zero error when the node is not shared by two or more elements, hence care must be taken before concluding the error. 3. This study does not throw any focus on accepted range of error, but gives fair idea about error estimation. Study can be further extended to get the range of accepted error values. 4. The methods discussed in the paper gives fair idea about importance of mesh convergence and methods of error estimation. This will help analyst to understand and analyze the results of his solution.
REFRENCES:
1. Finite element procedures Klaus-jurgen Bathe Prentice-Hall of India printed limited, New Delhi-110001 1997 2. Building better products with finite element analysis Vince Adams 3. NAFEMS A finite Element Primer 4. ANSYS 6 Documentation, (Online help).
