$$ (r _ {\theta} G) = 0. 0 0 3 7 5 \frac {1 2 \int_ {- t / 2} ^ {t / 2} G t ^ {2} d t}{t ^ {3}}. $$ For a general shell section defined by specifying the equivalent section properties directly, t is defined as $$ t = \sqrt {1 2 \frac {D _ {4 4} + D _ {5 5} + D _ {6 6}}{D _ {1 1} + D _ {2 2} + D _ {3 3}}} $$ and an effective shear modulus for the section is used to calculate the hourglass stiffness: $$ G = \frac {1}{6 t} (D _ {1 1} + D _ {2 2}) + \frac {1}{3 t} D _ {3 3}, $$ where $D _ { i j }$ is the section stiffness matrix. # User-defined hourglass stiffness When the initial shear modulus is not defined, you must define the hourglass stiffness parameters; an example is when user subroutine UMAT is used to describe the material behavior of elements with hourglassing modes. In some cases the default value provided for the hourglass control stiffness may not be suitable and you should define the value. In some coupled pore fluid diffusion and stress analyses the prevailing pore pressure in the medium may approach the magnitude of the stiffness of the material skeleton, as measured by constitutive parameters such as the elastic modulus. These cases are expected in some partial saturation evaluations of the wetting of relatively compliant materials such as tissues or cloth. When reduced-integration or modified tetrahedral or triangular elements are used in such analyses, the default choice of the hourglass control stiffness parameter, which is based on a scaling of skeleton material constitutive parameters, may not be adequate to control hourglassing in the presence of large pore pressure fields. An appropriate hourglass control stiffness in these cases should scale with the expected magnitude of pore pressure changes over an element. Input File Usage: Use the following option to specify nondefault values for the hourglass stiffness factors: \*HOURGLASS STIFFNESS $r _ { F } G , r _ { F } K , r _ { \theta } G _ { ; }$ , drilling hourglass scaling factor for shells This option must immediately follow one of the following options: \*MEMBRANE SECTION \*SHELL GENERAL SECTION \*SHELL SECTION \*SOLID SECTION Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Hourglass stiffness: Specify $r _ { F } G$ or for shells Membrane hourglass stiffness: Specify $r _ { F } G$ , Bending hourglass stiffness: Specify $r _ { \theta } G ,$ , and Drilling hourglass scaling factor: Specify drilling hourglass scaling factor for shells # Enhanced hourglass control approach in Abaqus/Standard and Abaqus/Explicit The enhanced hourglass control approach available in both Abaqus/Standard and Abaqus/Explicit represents a refinement of the pure stiffness method in which the stiffness coefficients are based on the enhanced assumed strain method; no scale factor is required. It is the default hourglass control approach for hyperelastic, hyperfoam, and low-density foam materials in Abaqus/Explicit and for hyperelastic, hyperfoam, and hysteresis materials in Abaqus/Standard. This method gives more accurate displacement solutions for coarse meshes with linear elastic materials as compared to other hourglass control methods. It also provides increased resistance to hourglassing for nonlinear materials. Although generally beneficial, this may give overly stiff response in problems displaying plastic yielding under bending. In Abaqus/Explicit the enhanced hourglass method will generally predict a much better return to the original configuration for hyperelastic or hyperfoam materials when loading is removed. The enhanced hourglass control approach is compatible between Abaqus/Standard and Abaqus/Explicit. It is recommended that enhanced hourglass control be used for both Abaqus/Standard and Abaqus/Explicit for all import analyses. See “Transferring results between Abaqus/Explicit and Abaqus/Standard,” Section 9.2.2. The enhanced hourglass method is not supported for enriched elements (see “Modeling discontinuities as an enriched feature using the extended finite element method,” Section 10.7.1). # Specifying the enhanced hourglass control approach The enhanced hourglass control method is available for first-order solid, membrane, and finite-strain shell elements with reduced integration. In Abaqus/Explicit it cannot be used for a hyperelastic or hyperfoam material when adaptive meshing is used on that domain (see the discussion below). Input File Usage: \*SECTION CONTROLS, NAME=name, HOURGLASS=ENHANCED Any scaling factors specified on the data line following this option will be ignored. Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Hourglass control: Enhanced Special considerations for hyperelastic and hyperfoam materials in an adaptive mesh domain in Abaqus/Explicit The enhanced hourglass method cannot be used with elements modeled with hyperelastic or hyperfoam materials that are included in an adaptive mesh domain. Thus, if you decide to use hyperelastic or hyperfoam materials in an adaptive mesh domain, you must specify section controls to choose a different hourglass control approach. The use of adaptive meshing in domains modeled with finite-strain elastic materials is not recommended since better results are generally predicted using the enhanced hourglass method and, for solid elements, element distortion control (discussed below). Therefore, for these materials it is recommended that the analysis be run without adaptive meshing but with enhanced hourglass control. Use in coupled pore pressure analysis When first-order, reduced-integration, or modified tetrahedral or triangular elements are used in coupled pore fluid diffusion and stress analyses or coupled temperature–pore pressure analyses with enhanced hourglass control, the hourglass control stiffness, which is based on skeleton material constitutive parameters, may not be adequate to control hourglassing in the presence of large pore pressure fields. Since enhanced hourglass control does not allow you to change the hourglass control stiffness, it is recommended that total stiffness hourglass control be used in these cases with an appropriate hourglass control stiffness scaled with the expected magnitude of pore pressure changes over an element. # Controlling element distortion for crushable materials in Abaqus/Explicit Many analyses with volumetrically compacting materials such as crushable foams see large compressive and shear deformations, especially when the crushable materials are used as energy absorbers between stiff or heavy components. The material behavior for crushable materials usually stiffens significantly under high compression. When a finer mesh is used, the stiffening behavior of the material model is enough to prevent excessive negative element volumes or other excessive distortion from occurring under high compressive loads. However, analyses may fail prematurely when the mesh is coarse relative to strain gradients and the amount of compression. Abaqus/Explicit offers distortion control to prevent solid elements from inverting or distorting excessively for these cases. The constraint method used in Abaqus/Explicit prevents each node on an element from punching inward toward the center of the element past a point where the element would become non-convex. Constraints are enforced by using a penalty approach, and you can control the associated distortion length ratio. Distortion control is available only for solid elements and cannot be used when the elements are included in an adaptive mesh domain. Distortion control is activated by default for elements modeled with hyperelastic, hyperfoam, or low-density foam materials. Using adaptive meshing in a domain modeled with hyperelastic or hyperfoam materials is not recommended since better results are generally predicted using the enhanced hourglass method in combination with element distortion control. However, if you decide to use hyperelastic or hyperfoam materials in an adaptive mesh domain, you must specify section controls to deactivate distortion control. When element distortion control is used in combination with the enhanced hourglass method (default behavior for hyperelastic and hyperfoam materials), a small amount of viscous damping is added to the element formulation and the associated viscous energy dissipation is included in the output of artificial strain energy (ALLAE). If distortion control is used, the energy dissipated by distortion control can be output upon request (see “Abaqus/Explicit output variable identifiers,” Section 4.2.2, for details). Although developed for analyses of energy absorbing, volumetrically compacting materials, distortion control can be used with any material model. However, care must be used in interpreting results since the distortion control constraints may inhibit legitimate deformation modes and lock up the mesh. Distortion control cannot prevent elements from being distorted due to temporal instabilities, hourglass instabilities, or physically unrealistic deformation.
Input File Usage:Use the following option to activate distortion control:*SECTION CONTROLS, NAME=name, DISTORTION CONTROL=YESUse the following option to deactivate distortion control:*SECTION CONTROLS, NAME=name, DISTORTION CONTROL=NO
Abaqus/CAE Usage:Mesh module: Mesh→Element Type: Distortion control: Yes or No
# Controlling the distortion length ratio By default, the constraint penalty forces are applied when the node moves to a point a small offset distance away from the actual plane of constraint. This appears to improve the robustness of the method and limits the reduction of time increment due to severe shortening of the element characteristic length. This offset distance is determined by the distortion length ratio times the initial element characteristic length. The default value of the distortion length ratio, r, is 0.1. You can change the distortion length ratio by specifying a value for $r , 0 < r \leq 1 \quad$ . Input File Usage: \*SECTION CONTROLS, NAME=name, DISTORTION CONTROL=YES, LENGTH RATIO=r Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Distortion control: Yes, Length ratio: r # Selecting a scale factor for the drill stiffness in Abaqus/Explicit A drill constraint acts to keep the element nodal rotations in the direction of the shell normal consistent with the average in-plane rotation of the element. Lack of such a constraint can lead to large rotations at these element nodes. Section controls can be used to select a scale factor for the default drill stiffness of an individual element set.
Input File Usage:Use the following options to specify a scale factor for the drill stiffness:*SECTION CONTROLS, NAME=name, , , , , , , , scale factor for drill stiffness
# Drill constraint in small strain shell elements S3RS and S4RS in Abaqus/Explicit The formulation of small strain shell elements S3RS and S4RS includes a drill constraint and does so by default. Alternatively, you can deactivate the drill constraint for these elements. The drill constraint is always active for the finite strain conventional shell elements such as S4R, but the default value of the drill stiffness can be scaled as mentioned above.
Input File Usage:Use the following option to activate the drill constraint (default):*SECTION CONTROLS, DRILL STIFFNESS=ONUse the following option to deactivate the drill constraint:*SECTION CONTROLS, DRILL STIFFNESS=OFF
# Ramping of initial stresses in membrane elements in Abaqus/Explicit For applications such as airbags in crash simulations the initial strains (hence, the initial stresses) are introduced into the model through a reference configuration that is different from the initial configuration. Often the components that confine the airbag in the initial configuration are excluded from the numerical model causing motion of the airbag under initial stresses at the beginning of the analysis. Abaqus/Explicit provides a technique to introduce the initial stresses in the membrane elements gradually based on an amplitude definition. This amplitude must be defined with its value starting from zero and reaching a final value of one. The initial stresses will not be applied for the duration that the amplitude stays at zero. Input File Usage: Use both of the following options: \*AMPLITUDE, NAME=name \*SECTION CONTROLS, RAMP INITIAL STRESS=name # Defining the kinematic formulation for hexahedron solid elements The default kinematic formulation for reduced-integration solid elements in Abaqus (and the only kinematic formulation available in Abaqus/Standard) is based on the uniform strain operator and the hourglass shape vectors. Details can be found in “Solid isoparametric quadrilaterals and hexahedra,” Section 3.2.4 of the Abaqus Theory Guide. These kinematic assumptions result in elements that pass the constant strain patch test for a general configuration and give zero strain under large rigid body rotation. However, the formulation is relatively expensive, especially in three dimensions. Abaqus/Explicit offers two alternative kinematic formulations for the C3D8R solid element that can reduce the computational cost. The performance for each kinematic formulation on the patch test and under large rigid body rotation for various element configurations is summarized in Table 27.1.4–1. Suitable applications for each kinematic formulation are summarized in Table 27.1.4–2. Table 27.1.4–1 Element performance for patch test and large rigid body rotations for various element configurations.
Element configurationKinematic formulation type
Average strainOrthogonalCentroid
Satisfaction of the three-dimensional patch testParallelepipedYesYesYes
GeneralYesNoNo
Zero straining under rigid body rotationParallelepipedYesYesYes
GeneralYesYesNo
Table 27.1.4–2 Different element formulations and their suitable applications. The default formulation is highlighted below.
Kinematic formulationOrder of accuracySuitable applications
Average strainSecond-orderAll; recommended for problems involving a large number of revolutions (>5).
Average strainFirst-orderAll; except those involving a large number of revolutions (>5).
Orthogonal—All; except those involving high confinement, very coarse meshes, or highly distorted elements.
Centroid—Problems with little rigid body rotation and reasonable mesh refinement.
You can specify the kinematic formulation for 8-node brick elements. # Default formulation The default average strain formulation of uniform strain and hourglass shape vectors is the only formulation available in Abaqus/Standard. This formulation is recommended for all problems and is particularly well suited for applications exhibiting high confinement, such as closed-die forming and bushing analyses. Input File Usage: \*SECTION CONTROLS, KINEMATIC SPLIT=AVERAGE STRAIN Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Kinematic split: Average strain # Orthogonal formulation in Abaqus/Explicit A noticeable reduction in computational cost can be obtained by using the orthogonal formulation available in Abaqus/Explicit. This formulation is based on the centroidal strain operator and a slight modification to the hourglass shape vectors. The centroidal strain operator requires three times fewer floating point operations than the uniform strain operator. Elements formulated with an orthogonal kinematic split pass the patch test only for rectangular or parallelepiped element configurations. However, numerical experience has shown that the element converges on the exact solution for general element configurations as the mesh is refined. It also performs well for large rigid body motions. This formulation provides a good balance between computational speed and accuracy. It is recommended for all analyses except those involving highly distorted elements, very coarse meshes, or high confinement. Suitable applications for this formulation include elastic drop testing. Input File Usage: \*SECTION CONTROLS, NAME=name, KINEMATIC SPLIT=ORTHOGONAL Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Kinematic split: Orthogonal # Centroid formulation in Abaqus/Explicit The fastest formulation available in Abaqus/Explicit is specified by selecting the centroid formulation. The centroid formulation is based on the centroidal strain operator and the hourglass base vectors. Using the hourglass base vectors instead of the hourglass shape vectors reduces hourglass mode computations by a factor of three. However, the hourglass base vectors are not orthogonal to rigid body rotation for general element configurations, so that hourglass strain may be generated with large rigid body rotations with this formulation. This formulation should be used only to improve computational performance on problems that have reasonable mesh refinement and no significant amount of rigid body rotation (e.g., transient flat rolling simulation). Input File Usage: \*SECTION CONTROLS, NAME=name, KINEMATIC SPLIT=CENTROID Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Kinematic split: Centroid # Choosing the order of accuracy in solid and shell element formulations Abaqus/Standard offers only a second-order accurate formulation for all elements. Abaqus/Explicit offers both first- and second-order accurate formulations for solid and shell elements. First-order accuracy is the default and yields sufficient accuracy for nearly all Abaqus/Explicit problems because of the inherently small time increment size. Second-order accuracy is usually required for analyses with components undergoing a large number of revolutions (>5). For three-dimensional solids the second-order accuracy formulation is available only with the default average strain kinematic formulation. # First-order accuracy In Abaqus/Explicit the first-order accurate formulation for solid and shell elements is the default. This formulation is not available in Abaqus/Standard. Input File Usage: \*SECTION CONTROLS, NAME=name, SECOND ORDER ACCURACY=NO Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Second-order accuracy: No # Second-order accuracy The second-order accurate element formulation is appropriate for problems with a large number of revolutions (>5). This is the only formulation available in Abaqus/Standard. “Simulation of propeller rotation,” Section 2.3.15 of the Abaqus Benchmarks Guide, illustrates the performance of second-order accurate shell and solid elements in Abaqus/Explicit as they undergo about 100 revolutions. Input File Usage: \*SECTION CONTROLS, NAME=name, SECOND ORDER ACCURACY=YES Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Second-order accuracy: Yes # Selecting scale factors for bulk viscosity in Abaqus/Explicit Bulk viscosity introduces damping associated with volumetric straining. Its purpose is to improve the modeling of high-speed dynamic events. Abaqus/Explicit contains two forms of bulk viscosity, linear and quadratic, which can be defined for the whole model at each step of the analysis, as discussed in “Bulk viscosity” in “Explicit dynamic analysis,” Section 6.3.3. Section controls can be used to select scale factors for the linear and quadratic bulk viscosities of an individual element set. The pressure term generated by bulk viscosity may introduce unexpected results in the volumetric response of highly compressible materials; therefore, it is recommended to suppress bulk viscosity for these materials by specifying scale factors equal to zero. Input File Usage: Use the following options to specify scale factors for the linear and quadratic bulk viscosities: \*SECTION CONTROLS, NAME=name , , , scale factor for linear bulk viscosity, scale factor for quadratic bulk viscosity Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Linear bulk viscosity scaling factor or Quadratic bulk viscosity scaling factor # Controlling element deletion and maximum degradation for materials with damage evolution Abaqus offers a general capability for modeling progressive damage and failure of materials (“Progressive damage and failure,” Section 24.1.1). In Abaqus/Standard this capability is available only for cohesive elements, connector elements, elements with plane stress formulations (plane stress, shell, continuum shell, and membrane elements), any element that can be used with the damage evolution models for ductile metals, and any element that can be used with the damage evolution law in a low-cycle fatigue analysis. In Abaqus/Explicit this capability is available for all elements with progressive damage behavior except connector elements. Section controls are provided to specify the value of the maximum stiffness degradation, $D _ { \mathrm { m a x } } .$ , and whether element deletion occurs when the degradation reaches this level. By default, an element is deleted when it is fully damaged (i.e., $D = D _ { \mathrm { m a x } } )$ . The choice of element deletion also affects how the damage is applied; details can be found in the following sections: • “Maximum degradation and choice of element removal” in “Damage evolution and element removal for ductile metals,” Section 24.2.3; • “Maximum degradation and choice of element removal in Abaqus/Standard” in “Connector damage behavior,” Section 31.2.7; • “Maximum degradation and choice of element removal” in “Defining the constitutive response of cohesive elements using a traction-separation description,” Section 32.5.6; • “Maximum degradation and choice of element removal” in “Damage evolution and element removal for fiber-reinforced composites,” Section 24.3.3; and • “Damage evolution for ductile materials in low-cycle fatigue,” Section 24.4.3.
Input File Usage:Use the following option to delete the element from the mesh:*SECTION CONTROLS, ELEMENT DELETION=YESUse the following option to keep the element in the computation:*SECTION CONTROLS, ELEMENT DELETION=NOUse the following option to specify $D_{\text{max}}$ :*SECTION CONTROLS, MAX DEGRADATION= $D_{\text{max}}$ .
Abaqus/CAE Usage:Use the following option to control whether completely damaged elements remain in the computation:Mesh module:Mesh→Element Type: Element deletionUse the following option to determine when an element is considered completely damaged:Mesh module:Mesh→Element Type: Max degradation
# Using viscous regularization with cohesive elements, connector elements, and elements that can be used with the damage evolution models for ductile metals and fiber-reinforced composites in Abaqus/Standard Material models exhibiting softening behavior and stiffness degradation often lead to severe convergence difficulties in implicit analysis programs, such as Abaqus/Standard. A common technique to overcome some of these convergence difficulties is the use of viscous regularization of the constitutive equations, which causes the tangent stiffness matrix of the softening material to be positive for sufficiently small time increments. The traction-separation laws used to describe the constitutive behavior of cohesive elements can be regularized in Abaqus/Standard using viscosity, by permitting stresses to be outside the limits defined by the traction-separation law. The details of the regularization procedure are discussed in “Viscous regularization in Abaqus/Standard” in “Defining the constitutive response of cohesive elements using a traction-separation description,” Section 32.5.6. The same technique is also used to regularize the following: • damaged (softening) connector response (see “Connector damage behavior,” Section 31.2.7), • damaged response of elements with plane stress formulations when they are used with the damage model for fiber-reinforced materials (see “Viscous regularization” in “Damage evolution and element removal for fiber-reinforced composites,” Section 24.3.3), and • damage response of elements used with the damage model for ductile metals (see “Damage evolution and element removal for ductile metals,” Section 24.2.3). You specify the amount of viscosity to be used for the regularization procedure. By default, no viscosity is included so that no viscous regularization is performed. Input File Usage: \*SECTION CONTROLS, VISCOSITY= Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Viscosity # Using viscous damping with connector elements in Abaqus/Standard Material failure in connector elements often causes convergence problems in Abaqus/Standard. To avoid such convergence problems, you can introduce viscous damping into the connector components by specifying the value of the damping coefficient as discussed in “Connector failure behavior,” Section 31.2.9. By default, no damping is included. Input File Usage: \*SECTION CONTROLS, VISCOSITY= Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Viscosity # Using section controls in an import analysis The recommended procedure for doing import analysis is to specify the enhanced hourglass control formulation in the original analysis. Once the section controls have been specified in the original analysis, they cannot be modified in subsequent import analyses. This ensures that the enhanced hourglass control formulation is used in the original as well as import analyses. The default values for other section controls are usually appropriate and should not be changed. For further details on using section controls in an import analysis, see “Transferring results between Abaqus/Explicit and Abaqus/Standard,” Section 9.2.2. # Using section controls for flexion-torsion type connector When the third axes of the two local coordinate systems for a flexion-torsion type connector are exactly aligned, a numerical singularity occurs that may lead to convergence difficulties. To avoid this, a small perturbation can be applied to the local coordinate system defined at the second connector node. Input File Usage: \*SECTION CONTROLS, PERTURBATION=small angle Abaqus/CAE Usage: You cannot specify a perturbation for flexion-torsion type connectors in Abaqus/CAE. # Using section controls to define the particle tracking box for DEM and SPH particles For discrete element method (DEM) analyses, a particle tracking box is established at the beginning of the analysis to define the rectangular region within which the particle search (finding all neighbors for all particles) is performed. A region that is 10% larger in all directions than the overall model initial dimensions and is centered at the geometric center of the model is used. For smoothed particle hydrodynamic (SPH) analyses, all particles are tracked as the analysis progresses by default. For DEM analyses, particle tracking is based on the initially established tracking box by default. Alternatively, you can define a particle tracking box to define the region within which the particle search is performed. You define a fixed size for the particle tracking box by specifying the coordinates of two opposite corners (lower left and upper right) of this box. As the analysis progresses, if a particle is outside this tracking box, it behaves like a free-flying point mass and does not contribute to the DEM or SPH calculations. If the particle reenters the box at a later stage, it is once again included in the calculations. If you want to track all of the particles during the analysis, you must ensure that the particle tracking box