3D element - Politecnico di Milano

FE analysis with 3D elements
E. Tarallo, G. Mastinu
POLITECNICO DI MILANO, Dipartimento di Meccanica
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)
3D element – topic
 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.
3D element – settings and problems (1)
 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
3D element – settings and problems (2)
 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
 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
3D Element recommendations (1)
For both Abaqus/Standard and Abaqus/Explicit:
1. Make all elements as “well shaped” as possible to improve convergence and
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.
3D Element recommendations (1)
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.
Exercise 1
Part: 3D solid homogeneus
Material: E=210 GPa, ν=0.3
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
Exercise 1 - results
Exercise 2
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
Exercise 2 - results
Exercise 3
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
Exercise 3 - results

similar documents