In ABAQUS/Standard section controls are used to select the enhanced hourglass control formulation for solid, shell, and membrane elements. This formulation provides improved coarse mesh accuracy with slightly higher computational cost and performs better for nonlinear material response at high strain levels when compared with the default total stiffness formulation. Section controls can also be used to select some element formulations that may be relevant for a subsequent ABAQUS/Explicit analysis.

In ABAQUS/Explicit the default formulations for solid, shell, and membrane elements have been chosen to perform satisfactorily on a wide class of quasi-static and explicit dynamic simulations. However, certain formulations give rise to some trade-off between accuracy and performance. ABAQUS/Explicit provides section controls to modify these element formulations so that you can optimize these objectives for a specific application. Section controls can also be used in ABAQUS/Explicit to specify scale factors for linear and quadratic bulk viscosity parameters.

In addition, section controls are used to specify the maximum stiffness degradation and to choose the behavior upon complete failure of an element, once the material stiffness is fully degraded, including the removal of failed elements from the mesh. This functionality applies only to elements with a material definition that includes progressive damage (see “Progressive damage and failure: overview,” Section 11.6.1, and “Defining the constitutive response of cohesive elements using a traction-separation description,” Section 18.5.6). In ABAQUS/Standard this functionality is limited to cohesive elements with a traction-separation constitutive response that includes damage evolution.

*SECTION CONTROLS, NAME=name

*MEMBRANE SECTION, CONTROLS=name
*SHELL GENERAL SECTION, CONTROLS=name
*SHELL SECTION, CONTROLS=name 
*SOLID SECTION, CONTROLS=name

The formulation for reduced-integration elements considers only the linearly varying part of the incremental displacement field in the element for the calculation of the increment of physical strain. The remaining part of the nodal incremental displacement field is the hourglass field and can be expressed in terms of hourglass modes. Excitation of these modes may lead to severe mesh distortion, with no stresses resisting the deformation. Hourglass control attempts to minimize this problem without introducing excessive constraints on the element's physical response.

The following methods are available in ABAQUS for suppressing the hourglass modes:

Integral viscoelastic approach in ABAQUS/Explicit

The integral viscoelastic approach available in ABAQUS/Explicit generates more resistance to hourglass forces early in the analysis step where sudden dynamic loading is more probable.

Let be an hourglass mode magnitude and be the force (or moment) conjugate to . The integral viscoelastic approach is defined as

where is the hourglass stiffness selected by ABAQUS/Explicit, and is one of up to three scaling factors , , and that you can define (by default, ). The scale factors are dimensionless and relate to specific displacement degrees of freedom. For solid and membrane elements scales all hourglass stiffnesses. For shell elements scales the hourglass stiffnesses related to the in-plane displacement degrees of freedom, and scales the hourglass stiffnesses related to the rotational degrees of freedom. In addition, scales the hourglass stiffness related to the transverse displacement for small-strain shell elements.

The integral viscoelastic form of hourglass control is available for all reduced-integration elements and is the default form in ABAQUS/Explicit, except for elements modeled with hyperelastic and hyperfoam materials. It is the most computationally intensive hourglass control method.

Input File Usage:

*SECTION CONTROLS, NAME=name, HOURGLASS=RELAX STIFFNESS , ,

ABAQUS/CAE Usage:

Mesh module: MeshElement Type: Hourglass control: Relax stiffness, Displacement hourglass scaling factor: , Rotational hourglass scaling factor: , Out-of-plane displacement hourglass scaling factor:

Kelvin viscoelastic approach in ABAQUS/Explicit

The Kelvin-type viscoelastic approach available in ABAQUS/Explicit is defined as

where is the linear stiffness and is the linear viscous coefficient. This general form has pure stiffness and pure viscous hourglass control as limiting cases. When the combination is used, the stiffness term acts to maintain a nominal resistance to hourglassing throughout the simulation and the viscous term generates additional resistance to hourglassing under dynamic loading conditions.

Three approaches are provided in ABAQUS/Explicit for specifying Kelvin viscoelastic hourglass control.

Specifying the pure stiffness approach

The pure stiffness form of hourglass control is available for all reduced-integration elements and is recommended for both quasi-static and transient dynamic simulations.

Input File Usage:

*SECTION CONTROLS, NAME=name, HOURGLASS=STIFFNESS , ,

ABAQUS/CAE Usage:

Mesh module: MeshElement Type: Hourglass control: Stiffness, Displacement hourglass scaling factor: , Rotational hourglass scaling factor: , Out-of-plane displacement hourglass scaling factor:

Specifying the pure viscous approach

The pure viscous form of hourglass control is available only for solid and membrane elements with reduced integration. It is the most computationally efficient form of hourglass control and has been shown to be effective for high-rate dynamic simulations. However, the pure viscous method is not recommended for low frequency dynamic or quasi-static problems since continuous (static) loading in hourglass modes will result in excessive hourglass deformation due to the lack of any nominal stiffness.

Input File Usage:

*SECTION CONTROLS, NAME=name, HOURGLASS=VISCOUS , ,

ABAQUS/CAE Usage:

Mesh module: MeshElement Type: Hourglass control: Viscous, Displacement hourglass scaling factor: , Rotational hourglass scaling factor: , Out-of-plane displacement hourglass scaling factor:

Specifying a combination of stiffness and viscous hourglass control

A linear combination of stiffness and viscous hourglass control is available only for solid and membrane elements with reduced integration. You can specify the blending weight factor () to scale the stiffness and viscous contributions. Specifying a weight factor equal to 0.0 or 1.0 results in the limiting cases of pure stiffness and pure viscous hourglass control, respectively. The default weight factor is 0.5.

Input File Usage:

*SECTION CONTROLS, NAME=name, HOURGLASS=COMBINED, WEIGHT FACTOR= , ,

ABAQUS/CAE Usage:

Mesh module: MeshElement Type: Hourglass control: Combined, Stiffness-viscous weight factor: , Displacement hourglass scaling factor: , Rotational hourglass scaling factor: , Out-of-plane displacement hourglass scaling factor:

Total stiffness approach in ABAQUS/Standard

The total stiffness approach available in ABAQUS/Standard is the default hourglass control approach for all first-order, reduced-integration elements in ABAQUS/Standard, except for elements modeled with hyperelastic, hyperfoam, or hysteresis materials. It is the only hourglass control approach available in ABAQUS/Standard for S8R5, S9R5, and M3D9R elements. It is based on hourglass stiffness factors that depend on the shear modulus and are constant for the entire model. A scale factor can be applied to these stiffness factors to increase or decrease the hourglass stiffness.

Let be an hourglass mode magnitude and be the force (or moment) conjugate to . The total stiffness approach for hourglass control in membrane or solid elements or membrane hourglass control in shell elements is defined as

where is a dimensionless scale factor (by default, ); is an hourglass stiffness factor with units of stress; is the gradient interpolator used to define constant gradients in the element ( where the superscript refers to an element node, the subscript refers to a direction, and is a material coordinate); and is the element volume. Similarly, for bending hourglass control in shell elements the total stiffness approach is defined as

where is the scale factor (by default, ), is the hourglass stiffness factor, is the thickness of the shell element, and is the area of the shell element.

Input File Usage:

*SECTION CONTROLS, NAME=name, HOURGLASS=STIFFNESS ,

ABAQUS/CAE Usage:

Mesh module: MeshElement Type: Hourglass control: Stiffness, Displacement hourglass scaling factor: , Rotational hourglass scaling factor:

Default hourglass stiffness values

Normally the hourglass control stiffness is defined from the elasticity associated with the material. In most cases it is based on a typical value of the initial shear modulus of the material, which may, for example, be given as part of the elastic material definition (“Linear elastic behavior,” Section 10.2.1). For an isotropic elastic or hyperelastic material is the shear modulus. For a nonisotropic elastic material an average shear modulus is used to calculate the hourglass stiffness: for orthotropic elasticity defined by specifying the terms in the elastic stiffness matrix or for anisotropic elasticity

and for orthotropic elasticity defined by specifying the engineering constants or for orthotropic elasticity in plane stress

If the elastic moduli are dependent on temperature or field variables, the first value in the table is used. The default values for the stiffness factors are defined below.

For membrane or solid elements

For membrane hourglass control in a shell

For control of bending hourglass modes in a shell

For a general shell section defined by specifying the equivalent section properties directly, is defined as

and an effective shear modulus for the section is used to calculate the hourglass stiffness:

where 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 (“UMAT,” Section 25.2.30) 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 element is 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 , , , drilling hourglass scaling factor for shells This option must immediately follow one of the following options: *MEMBRANE SECTION, CONTROLS=name *SHELL GENERAL SECTION, CONTROLS=name *SHELL SECTION, CONTROLS=name *SOLID SECTION, CONTROLS=name

ABAQUS/CAE Usage:

Mesh module: MeshElement Type: Hourglass stiffness: Specify or for shells Membrane hourglass stiffness: Specify , Bending hourglass stiffness: Specify , and Drilling hourglass scaling factor: Specify drilling hourglass scaling factor for shells

*SECTION CONTROLS, NAME=name, HOURGLASS=ENHANCED

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 or hyperfoam 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.

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.

*SECTION CONTROLS, NAME=name, DISTORTION CONTROL=YES

*SECTION CONTROLS, NAME=name, DISTORTION CONTROL=NO

*SECTION CONTROLS, NAME=name,  DISTORTION CONTROL=YES, 
LENGTH RATIO=

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 Manual. 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 13.1.4–1. Suitable applications for each kinematic formulation are summarized in Table 13.1.4–2.

You can specify the kinematic formulation for 8-node brick elements.

*SECTION CONTROLS, KINEMATIC SPLIT=AVERAGE STRAIN

*SECTION CONTROLS, NAME=name, 
KINEMATIC SPLIT=ORTHOGONAL

*SECTION CONTROLS, NAME=name, KINEMATIC SPLIT=CENTROID

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.

*SECTION CONTROLS, NAME=name, 
SECOND ORDER ACCURACY=NO

*SECTION CONTROLS, NAME=name, 
SECOND ORDER ACCURACY=YES

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, such as low density foams; therefore, it is recommended to suppress bulk viscosity for these materials by specifying scale factors equal to zero.

*SECTION CONTROLS, NAME=name
 , , , scale factor for linear bulk viscosity, scale factor for quadratic bulk viscosity

ABAQUS offers a general capability for modeling progressive damage and failure of materials (“Progressive damage and failure: overview,” Section 11.6.1). In ABAQUS/Standard this capability can be used only with cohesive elements. Section controls are provided to specify the value of the maximum stiffness degradation, , and whether element deletion occurs when the degradation reaches this level. By default, an element is deleted when it is fully damaged (i.e., ). The choice of element deletion also affects how the damage is applied; details can be found in “Maximum degradation and choice of element removal” in “Damage evolution and element removal,” Section 11.6.3, and in “Maximum degradation and choice of element removal” in “Defining the constitutive response of cohesive elements using a traction-separation description,” Section 18.5.6.

*SECTION CONTROLS, ELEMENT DELETION=YES

*SECTION CONTROLS, ELEMENT DELETION=NO

*SECTION CONTROLS, MAX DEGRADATION=.

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 18.5.6. 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.

*SECTION CONTROLS, VISCOSITY=

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 7.7.2.