#### Transcript 3D element - Politecnico di Milano

FE analysis with 3D elements E. Tarallo, G. Mastinu POLITECNICO DI MILANO, Dipartimento di Meccanica Summary 2 Subjects covered in this tutorial An introduction to 3D elements Formulations and problems of solid continuum elements A guided example to evaluate a simple structure through the use of FEM Comparison between standard and explicit solver Other few exercises (to include in exercises-book) Es02 Es-04 3D element – topic 3 The solid element library includes isoparametric elements: quadrilaterals in two dimensions and “bricks” (hexahedra) in three dimensions. These isoparametric elements are generally preferred for most cases because they are usually the more cost-effective of the elements that are provided in Abaqus. They are offered with first- and second-order interpolation Standard first-order elements are essentially constant strain elements: the isoparametric forms can provide more than constant strain response, but the higher-order content of the solutions they give is generally not accurate and, thus, of little value. The second-order elements are capable of representing all possible linear strain fields. Thus, in the case of many problems (elasticity, heat conduction, acoustics) much higher solution accuracy per degree of freedom is usually available with the higher-order elements. Therefore, it is generally recommended that the highest-order elements available be used for such cases: in Abaqus this means second-order elements. Es02 Es-04 3D element – settings and problems (1) 4 FULL or REDUCED INTEGRATION: reduced integration uses a lower-order integration to form the element stiffness. The mass matrix and distributed loadings use full integration. Reduced integration reduces running time, especially in three dimensions. For example, element type C3D20 has 27 integration points, while C3D20R has only 8; therefore, element assembly is roughly 3.5 times more costly for C3D20 than for C3D20R (use only with hexahedra elements). HOURGLASS: hourglassing can be a problem with first-order, reduced-integration elements (CPS4R, CAX4R, C3D8R, etc.) in stress/displacement analyses. Since the elements have only one integration point, it is possible for them to distort in such a way that the strains calculated at the integration point are all zero, which, in turn, leads to uncontrolled distortion of the mesh. Countermeasure: use finer mesh SHEAR & VOLUMETRIC LOCKING: Shear locking occurs in first-order, fully integrated elements (CPS4, CPE4, C3D8, etc.) that are subjected to bending. The numerical formulation of the elements gives rise to shear strains that do not really exist—the so-called parasitic shear (elements too stiff in bending) Countermeasure: use finer mesh through the thickness of the section Es02 Es-04 3D element – settings and problems (2) 5 HYBRID FORMULATION: Hybrid elements are intended primarily for use with incompressible and almost incompressible material behavior; these elements are available only in Abaqus/Standard. When the material response is incompressible, the solution to a problem cannot be obtained in terms of the displacement history only, since a purely hydrostatic pressure can be added without changing the displacements. INCOMPATIBLE MODE: Incompatible mode elements (CPS4I, CPE4I, CAX4I, CPEG4I, and C3D8I and the corresponding hybrid elements) are first-order elements that are enhanced by incompatible modes to improve their bending behavior. In addition to the standard displacement degrees of freedom, incompatible deformation modes are added internally to the elements. The primary effect of these modes is to eliminate the parasitic shear stresses that cause the response of the regular first-order displacement elements to be too stiff in bending. Because of the added internal degrees of freedom due to the incompatible modes (4 for CPS4I; 5 for CPE4I, CAX4I, and CPEG4I; and 13 for C3D8I), these elements are somewhat more expensive than the regular first-order displacement elements; however, they are significantly more economical than second-order elements. The incompatible mode elements use full integration and, thus, have no hourglass modes. Es02 Es-04 3D Element recommendations (1) 6 For both Abaqus/Standard and Abaqus/Explicit: 1. Make all elements as “well shaped” as possible to improve convergence and accuracy. 2. If an automatic tetrahedral mesh generator is used, use the second-order elements C3D10 (in Abaqus/Standard) or C3D10M (in Abaqus/Explicit). 3. If contact is present in Abaqus/Standard, use the modified tetrahedral element C3D10M if the default “hard” contact relationship is used or in analyses with large amounts of plastic deformation. 4. If possible, use hexahedral elements in three-dimensional analyses since they give the best results for the minimum cost. Es02 Es-04 3D Element recommendations (1) 7 For only Abaqus/Standard: 1. For linear and “smooth” nonlinear problems use reduced-integration, secondorder elements if possible. 2. Use second-order, fully integrated elements close to stress concentrations to capture the severe gradients in these regions. However, avoid these elements in regions of finite strain if the material response is nearly incompressible. 3. Use first-order quadrilateral or hexahedral elements or the modified triangular and tetrahedral elements for problems involving contact or large distortions. If the mesh distortion is severe, use reduced-integration, first-order elements. 4. If the problem involves bending and large distortions, use a fine mesh of firstorder, reduced-integration elements. 5. Hybrid elements must be used if the material is fully incompressible (except when using plane stress elements). Hybrid elements should also be used in some cases with nearly incompressible materials. 6. Incompatible mode elements can give very accurate results in problems dominated by bending. Es02 Es-04 Exercise 1 8 Part: 3D solid homogeneus Material: E=210 GPa, ν=0.3 Problem: 1. Perform static analysis 2. Find max deflection 3. Evaluate von mises stress changing the mesh (number and order of elements) 4. Perform dynamic analysis (0.005 s time step, 125 equally spaced interval save output) NB: density [kg/mm3]; E [kg/mm/s2] 5. Plot Internal energy, kinetic energy and displacement vs time Es02 Es-04 Exercise 1 - results 9 Es02 Es-04 Exercise 2 10 Fz Fy Material: E=210 GPa, ν=0.3 Load: Fz=5kN; Fy=3kN; T=100kNmm Analysis: Static Element: compare different elements Problem: find max von mises stresses on the notches Es02 Es-04 Exercise 2 - results 11 Es02 Es-04 Exercise 3 12 Material: E=210 GPa, ν=0.3 Load: F=30kN Analysis: Static Element: use partition to mesh with HEX linear or quadratic Problem: find max von mises stresses on the notches Es02 Es-04 Exercise 3 - results 13 Es02 Es-04