Section Controls

Using Section Controls

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 might 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. You can also control the initial stresses in membrane elements for applications such as airbags in crash simulations and introduce the initial stresses gradually based on an amplitude definition.

In addition, section controls are used to specify the maximum stiffness degradation and to choose the behavior on 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 About Progressive Damage and Failure, Connector Damage Behavior, and Defining the Constitutive Response of Cohesive Elements Using a Traction-Separation Description). In Abaqus/Standard this functionality is limited to

cohesive elements with a traction-separation constitutive response that includes damage evolution,
any element with a plane stress formulation that can be used with the damage evolution model for fiber-reinforced composites,
any element that can be used with the damage evolution models for ductile metals,
any element that can be used with the damage evolution law in a low-cycle fatigue analysis, and
connector elements with a constitutive response that includes damage evolution.

Input File Usage

Use the following option to specify a section controls definition:

SECTION CONTROLS, NAME=name

This option is used in conjunction with one or more of the following options to associate the section control definition with an element section definition:

COHESIVE SECTION, CONTROLS=name
CONNECTOR SECTION, CONTROLS=name
DISCRETE SECTION, CONTROLS=name
EULERIAN SECTION, CONTROLS=name
MEMBRANE SECTION, CONTROLS=name
SHELL GENERAL SECTION, CONTROLS=name
SHELL SECTION, CONTROLS=name 
SOLID SECTION, CONTROLS=name

You can apply a single section control definition to several element section definitions.

Abaqus/CAE Usage

Mesh module: MeshElement Type: Element Controls

Methods for Suppressing Hourglass Modes

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 might lead to severe mesh distortion, with no stresses resisting the deformation. Similarly, the formulation for element type C3D4H considers in the constraint equations only the constant part of the incremental pressure Lagrange multiplier field. The remaining part of the nodal incremental pressure Lagrange multiplier interpolation is comprised of hourglass modes.

Hourglass control attempts to minimize these problems without introducing excessive constraints on the element's physical response.

Several methods are available in Abaqus for suppressing the hourglass modes, as described below.

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

Q = \int_{0}^{t} s K (t - t^{​^{'}}) \frac{d q}{d t^{​^{'}}} d t^{​^{'}},

where K is the hourglass stiffness selected by Abaqus/Explicit, and s is one of up to three scaling factors $s^{s}$ , $s^{r}$ , and $s^{w}$ that you can define (by default, $s^{s} = s^{r} = s^{w} = 1.0$ ). The scale factors are dimensionless and relate to specific displacement degrees of freedom. For solid elements $s^{s}$ scales all hourglass stiffnesses. For membrane elements $s^{s}$ scales the hourglass stiffnesses related to the in-plane displacement degrees of freedom, and $s^{w}$ scales the out-of-plane displacement degrees of freedom. For shell elements $s^{s}$ scales the hourglass stiffnesses related to the in-plane displacement degrees of freedom, and $s^{r}$ scales the hourglass stiffnesses related to the rotational degrees of freedom. In addition, $s^{w}$ 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, hyperfoam, and low-density foam materials and for Eulerian EC3D8R elements. It is the most computationally intensive hourglass control method. It is not supported for Eulerian EC3D8R elements.

Input File Usage

SECTION CONTROLS, NAME=name, 
HOURGLASS=RELAX STIFFNESS
 $s^{s}$ ,  $s^{r}$ ,  $s^{w}$

Abaqus/CAE Usage

Mesh module: MeshElement Type: Hourglass control: Relax stiffness, Displacement hourglass scaling factor:  $s^{s}$ , Rotational hourglass scaling factor:  $s^{r}$ , Out-of-plane displacement hourglass scaling factor:  $s^{w}$

Kelvin Viscoelastic Approach in Abaqus/Explicit

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

Q = s [(1 - α) K q + α C \frac{d q}{d t}],

where K is the linear stiffness and C 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
 $s^{s}$ ,  $s^{r}$ ,  $s^{w}$

Abaqus/CAE Usage

Mesh module: MeshElement Type: Hourglass control: Stiffness, Displacement hourglass scaling factor:  $s^{s}$ , Rotational hourglass scaling factor:  $s^{r}$ , Out-of-plane displacement hourglass scaling factor:  $s^{w}$

Specifying the Pure Viscous Approach

The pure viscous form of hourglass control is available only for solid and membrane elements with reduced integration and is the default form in Abaqus/Explicit for Eulerian EC3D8R elements. 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 results in excessive hourglass deformation due to the lack of any nominal stiffness.

Input File Usage

SECTION CONTROLS, NAME=name, HOURGLASS=VISCOUS
 $s^{s}$ ,  $s^{r}$ ,  $s^{w}$

Abaqus/CAE Usage

Mesh module: MeshElement Type: Hourglass control: Viscous, Displacement hourglass scaling factor:  $s^{s}$ , Rotational hourglass scaling factor:  $s^{r}$ , Out-of-plane displacement hourglass scaling factor:  $s^{w}$

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 $α$ ( $0 \leq α \leq 1$ ) 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= $α$ 
 $s^{s}$ ,  $s^{r}$ ,  $s^{w}$

Abaqus/CAE Usage

Mesh module: MeshElement Type: Hourglass control: Combined, Stiffness-viscous weight factor:  $α$ , Displacement hourglass scaling factor:  $s^{s}$ , Rotational hourglass scaling factor:  $s^{r}$ , Out-of-plane displacement hourglass scaling factor:  $s^{w}$

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 and the only hourglass control approach available for the pressure Lagrange multiplier interpolation for C3D4H elements. Hourglass stiffness factors for first-order, reduced-integration elements depend on the shear modulus, while factors for C3D4H elements depend on the bulk modulus. A scale factor can be applied to these stiffness factors to increase or decrease the hourglass stiffness.

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

Q = s^{s} ((r_{F} G) B_{α}^{P} B_{α}^{P} V) q,

where $s^{s}$ is a dimensionless scale factor (by default, $s^{s} = 1.0$ ); $r_{F} G$ is an hourglass stiffness factor with units of stress; $B_{α}^{P}$ is the gradient interpolator used to define constant gradients in the element ( $\partial u / \partial S_{α} = B_{α}^{P} u^{P},$ where the superscript P refers to an element node, the subscript $α$ refers to a direction, and $S_{α}$ is a material coordinate); and V is the element volume. Similarly, the hourglass control for the pressure Lagrange multiplier interpolation for C3D4H elements is defined as

Q = s^{p} ((r_{F} K) B^{P} B^{P} V) q,

where $s^{p}$ is a dimensionless scale factor (by default, $s^{p} = 1.0$ ); $B^{P}$ is a volumetric gradient operator; and $r_{F} K$ is an hourglass stiffness factor with units of stress for compressible hyperelastic and hyperfoam materials and units of stress compliance for all other materials. The total stiffness approach for bending hourglass control in shell elements is defined as

Q = s^{r} ((r_{θ} G) B_{α}^{P} B_{α}^{P} t^{3} A) q,

where $s^{r}$ is the scale factor (by default, $s^{r} = 1.0$ ), $r_{θ} G$ is the hourglass stiffness factor, t is the thickness of the shell element, and A is the area of the shell element.

Input File Usage

SECTION CONTROLS, NAME=name, HOURGLASS=STIFFNESS
 $s^{s}$ ,  $s^{r}$ , , , ,  $s^{p}$

Abaqus/CAE Usage

Mesh module: MeshElement Type: Hourglass control: Stiffness, Displacement hourglass scaling factor:  $s^{s}$ , Rotational hourglass scaling factor:  $s^{r}$

Default Hourglass Stiffness Values

Normally the hourglass control stiffness is defined from the elasticity associated with the material. In most cases, the control stiffness of first-order, reduced-integration elements is based on a typical value of the initial shear modulus of the material, which might, for example, be given as part of the elastic material definition (Linear Elastic Behavior). Similarly, hourglass control stiffness of the reduced-integration pressure and volumetric Lagrange multiplier interpolations of C3D4H elements is based on a typical value of the initial bulk modulus. For an isotropic elastic or hyperelastic material G is the shear modulus. For a nonisotropic elastic material average moduli are used to calculate the hourglass stiffness: for orthotropic elasticity defined by specifying the terms in the elastic stiffness matrix or for anisotropic elasticity

G = \frac{1}{3} (D_{1212} + D_{1313} + D_{2323})

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

G = \frac{1}{3} (G_{12} + G_{13} + G_{23}) .

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

(r_{F} G) = 0.005 G .

For membrane hourglass control in a shell

(r_{F} G) = 0.005 \frac{\int_{- t / 2}^{t / 2} G d t}{t} .

For control of bending hourglass modes in a shell

(r_{θ} G) = 0.00375 \frac{12 \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{12 \frac{D_{44} + D_{55} + D_{66}}{D_{11} + D_{22} + D_{33}}}

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

G = \frac{1}{6 t} (D_{11} + D_{22}) + \frac{1}{3 t} D_{33},

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 might 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 might 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, might 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
 $r_{F} G$ ,  $r_{F} K$ ,  $r_{θ} G$ , 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: MeshElement Type: Hourglass stiffness: Specify  $r_{F} G$  or for shells Membrane hourglass stiffness: Specify  $r_{F} G$ , Bending hourglass stiffness: Specify  $r_{θ} G$ , 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 might 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.

The enhanced hourglass method is not supported for enriched elements (see Modeling Discontinuities as an Enriched Feature Using the Extended Finite Element Method).

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: MeshElement 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, might 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 negative element volumes or other excessive distortion from occurring under high compressive loads. However, analyses might 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, crushable foam, or low-density foam materials when the default hourglass control method is used. If you decide to use any of these materials with solid elements included in an adaptive mesh domain, you must specify section controls to deactivate distortion control. 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.

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 on request (see Abaqus/Explicit Output Variable Identifiers 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 might 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=YES

Use the following option to deactivate distortion control:

SECTION CONTROLS, NAME=name, DISTORTION CONTROL=NO

Abaqus/CAE Usage

Mesh module: MeshElement 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, $0 < r \leq 1$ .

For C3D10 elements, instead of the distortion length ratio, the distortion volume ratio (the current volume over the original volume at each integration point) is used. The default threshold value of the distortion volume ratio, r, is also 0.1. You can change the distortion volume ratio by specifying a value for r, $0 < r \leq 1$ .

Input File Usage

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

Abaqus/CAE Usage

Mesh module: MeshElement 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=ON

Use the following option to deactivate the drill constraint:

SECTION CONTROLS, DRILL STIFFNESS=OFF

Ramping of Initial Stresses in Abaqus/Explicit

Abaqus/Explicit provides a technique to introduce initial stresses gradually based on an amplitude definition to reduce possible oscillations in the initial solution. You must define this amplitude with a value starting from zero and reaching a final value of one. The initial stresses are not applied for the duration that the amplitude stays at zero, and the incurred energy for the duration that the amplitude is greater than zero is added to the system through output variable ALLVD. This technique is available with solid elements, membrane elements, beam elements, and shell elements (S4R and S4RS).

You can use the ramping technique in combination with user-defined initial stresses (see Defining Initial Stresses) or together with a reference mesh definition (see Defining a Reference Mesh for Membrane Elements and Three-Dimensional Solid Elements).

In crash-related simulations (such as airbag deployment or dummy positioning/settling), the initial stresses are often introduced in the model through the definition of a reference configuration that is different from the initial configuration. For airbag modeling, the components that confine the airbag in the initial configuration are often excluded from the numerical model, which might cause motion of the airbag under initial stresses at the beginning of the analysis. For dummy positioning/settling modeling, the initial stresses introduced by the reference mesh might cause initial oscillations in the solution. By ramping the initial stresses, you can avoid or reduce the initial motion of the airbag and the initial oscillations.

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

Table 1. Element performance for patch test and large rigid body rotations for various element configurations.
	Element configuration	Kinematic formulation type
	Element configuration	Average strain	Orthogonal	Centroid
Satisfaction of the three-dimensional patch test	Parallelepiped	Yes	Yes	Yes
Satisfaction of the three-dimensional patch test	General	Yes	No	No
Zero straining under rigid body rotation	Parallelepiped	Yes	Yes	Yes
Zero straining under rigid body rotation	General	Yes	Yes	No

Table 2. Different element formulations and their suitable applications. The default formulation is highlighted below.
Kinematic formulation	Order of accuracy	Suitable applications
Average strain	Second-order	All; recommended for problems involving a large number of revolutions (>5).
Average strain	First-order	All; 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: MeshElement 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: MeshElement 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 might 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 (for example, transient flat rolling simulation).

Input File Usage

SECTION CONTROLS, NAME=name, KINEMATIC SPLIT=CENTROID

Abaqus/CAE Usage

Mesh module: MeshElement 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: MeshElement 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 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: MeshElement 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. 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 might 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: MeshElement Type: Linear bulk viscosity scaling factor or Quadratic bulk viscosity scaling factor

Controlling the Activation of the "Improved" Element Time Estimation Method in Abaqus/Explicit

For three-dimensional continuum elements and elements with plane stress formulations (shell, membrane, and two-dimensional plane stress elements) an "improved" estimate of the element characteristic length is used by default. This "improved" method usually results in a larger element stable time increment than a more traditional method. The activation of the "improved" element time estimation method can be defined globally for the whole model at each step of the analysis, as discussed in Time Incrementation. Alternatively, you can selectively control the activation of the "improved" element time estimation method for each individual element set.

Input File Usage

Use the following option to match the setting of the "improved" element time estimation method defined globally for the whole model:

SECTION CONTROLS, NAME=name, 
IMPROVED DT METHOD=GLOBAL

Use the following option to activate the "improved" element time estimation method:

SECTION CONTROLS, NAME=name, 
IMPROVED DT METHOD=YES

Use the following option to deactivate the "improved" element time estimation method:

SECTION CONTROLS, NAME=name, 
IMPROVED DT METHOD=NO

Abaqus/CAE Usage

Controlling the activation of the "improved" element time estimation method is not supported in Abaqus/CAE.

Controlling Element Deletion and Maximum Degradation for Materials with Damage Evolution

Abaqus offers a general capability for modeling progressive damage and failure of materials (About Progressive Damage and Failure). 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, $D_{\max}$ , for material failure and whether element deletion occurs when the degradation reaches this level. By default, an element is deleted on material failure. Details for element deletion driven by material failure are described in Material Failure and Element Deletion. The choice of element deletion also affects how the damage is applied; details can be found in the following sections:

Input File Usage

Use the following option to delete the element from the mesh:

SECTION CONTROLS, ELEMENT DELETION=YES

Use the following option to keep the element in the computation:

SECTION CONTROLS, ELEMENT DELETION=NO

Use the following option to specify $D_{\max}$ :

SECTION CONTROLS, MAX DEGRADATION= $D_{\max}$

Abaqus/CAE Usage

Use the following option to control whether completely damaged elements remain in the computation:

Mesh module: MeshElement Type: Element deletion

Use the following option to determine when an element is considered completely damaged:

Mesh module: MeshElement Type: Max degradation

Controlling Shell Element Deletion Based on Integration Point Status in Abaqus/Explicit

In Abaqus/Explicit you can delete shell elements based on the number of active or failed integration points through the shell section. By default, when only one integration point through the shell section is active, the shell element is deleted. You can specify either the number of active integration points or the number of failed integration points through the shell section at which the shell element is deleted. The number you specify must not exceed the total number of integration points through the shell section. Alternatively, you can specify that a shell element is deleted when all of the integration points through the shell section are failed.

Input File Usage

Use the following option to specify the number of active integration points through the shell section at which the shell element is deleted:

SECTION CONTROLS, SHELL DELETION NUMBER=positive integer

Use the following option to specify the number of failed integration points through the shell section at which the shell element is deleted:

SECTION CONTROLS, SHELL DELETION NUMBER=negative integer

Use the following option to delete the shell element when all of the integration points through the shell section are failed:

SECTION CONTROLS, SHELL DELETION NUMBER=0

Abaqus/CAE Usage

Controlling shell element deletion based on integration point status is not supported in Abaqus/CAE.

Controlling Distortion-Based Element Deletion in Abaqus/Explicit

In Abaqus/Explicit you can control element deletion for deformable elements (except cohesive elements) based on distortion. An inherent limit exists as to how much deformation a Lagrangian element can accommodate to obtain accurate simulation results. By default, elements are deleted only when material failure is defined and failure occurs. In rare cases, an element can become excessively distorted before material failure occurs and cause the simulation to stop prematurely. In addition, when an element gets distorted, the element stable time increment can drop dramatically, causing a performance issue. You can activate distortion-based element deletion to delete the distorted elements and allow the simulation to continue.

You can control the deletion of distorted elements using the following measures: current element stable time increment, volume or area, or characteristic length. The element stable time increment used does not include damping (bulk viscosity), mass scaling, or penalty contact effects. The element is removed once the measure falls below the specified value. The deletion criteria can be based on a ratio of the deletion measure over the original value; for example, the ratio of the element volume over the original element volume at which the element is deleted. Alternatively, you can specify a value for the deletion measure; for example, the element volume at which the element is deleted.

Distortion-based element deletion is intended for experienced users and should be used with caution. Setting improper values for the deletion criteria can lead to unphysical or misleading results.

Input File Usage

Use the following option to activate distortion-based element deletion and to specify the associated distortion criteria:

SECTION CONTROLS, DELETE DISTORTED ELEMENT=YES
first data line
second data line
third data line
fourth data line
fifth data line
stable time increment ratio, volume or area ratio, characteristic length ratio, stable time increment, 
volume or area, characteristic length

Abaqus/CAE Usage

Controlling distortion-based element deletion is not supported in Abaqus/CAE.

Using Linear Kinematic Conversion in Abaqus/Explicit

When elements are subject to large compressive forces, they can reach a point when negative volumes are calculated. The negative volumes cause a fatal error if nonlinear geometric effects are considered. One method to avoid the fatal error is to convert the element from nonlinear kinematics to linear kinematics when it reaches a certain level of compression (volume reduction).

Linear kinematic conversion is activated only when distortion control is also activated. The element is converted when distortion control forces become active. For C3D10 elements, linear kinematic conversion does not require the use of distortion control. For C3D10 elements, linear kinematic conversion occurs when the ratio of the element characteristic length over the original characteristic length reaches a critical value.

Linear kinematic conversion allows the simulation to continue subject to approximation of linear kinematics for the highly distorted elements. Linear kinematic conversion can be used as an alternative to distortion-based element deletion (see Controlling Distortion-Based Element Deletion in Abaqus/Explicit).

The linear kinematic conversion is mainly developed to improve element robustness. The element computation results will not be exactly accurate for the elements that have been converted to linear kinematics. Therefore, linear kinematic conversion should be used with caution to avoid unphysical or misleading results.

Input File Usage

Use the following option to activate linear kinematic conversion:

SECTION CONTROLS, LINEAR KINEMATIC CONVERSION

Abaqus/CAE Usage

Controlling linear kinematic conversion is not supported in Abaqus/CAE.

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. The same technique is also used to regularize the following:

damaged (softening) connector response (see Connector Damage Behavior),
damaged response of elements with plane stress formulations when they are used with the damage model for fiber-reinforced materials (see Viscous Regularization), and
damage response of elements used with the damage model for ductile metals (see Damage Evolution and Element Removal for Ductile Metals).

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= $μ$

Abaqus/CAE Usage

Mesh module: MeshElement Type: Viscosity

Using Section Controls for Slurry Transport in Abaqus/Standard

In slurry transport analysis in Abaqus/Standard, slurry concentration is represented by the volumetric fraction of particles in a homogenized way. Although the particles are not tracked explicitly, you can control if particles are allowed to move into a fracture by specifying a minimum ratio, $α$ , between the crack width and particle diameter. Particles can only move into a fracture with a gap opening of at least $α$ times the particle diameter. By default, the minimum ratio $α$ is 1.0.

Input File Usage

SECTION CONTROLS, MIN GAP PARTICLE RATIO= $α$

Abaqus/CAE Usage

You cannot specify a minimum gap particle ratio in Abaqus/CAE.

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. By default, no damping is included.

Input File Usage

SECTION CONTROLS, VISCOSITY= $μ$

Abaqus/CAE Usage

Mesh module: MeshElement 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.

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 might 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 fully encompasses the domain through which the model moves; otherwise, you will lose tracking of the particle.

Input File Usage

Use the following option to specify a fixed size for the particle tracking box in a DEM analysis:

SECTION CONTROLS
blank line
blank line
X, Y, and Z-coordinates (lower box corner) and X, Y, and Z-coordinates
(upper box corner)

Use the following option to specify a fixed size for the particle tracking box in an SPH analysis:

SECTION CONTROLS
first data line
second data line
X, Y, and Z-coordinates (lower box corner) and X, Y, and Z-coordinates
(upper box corner), 0

Abaqus/CAE Usage

In Abaqus/CAE you can only specify section controls for SPH parameters in Abaqus/Explicit analyses involving the conversion of continuum elements to SPH particles.

Using Section Controls for Smoothed Particle Hydrodynamics (SPH)

In addition to controlling the size of the particle tracking box, you can control other aspects of the smoothed particle hydrodynamic (SPH) formulation implemented in Abaqus/Explicit.

Using Section Controls for Specifying the SPH Kernel

For a smoothed particle hydrodynamic analysis, you can choose the order of the kernel used for interpolation. For a list of references that discuss the various kernels that can be used, see Smoothed Particle Hydrodynamics.

Input File Usage

Use one of the following options:

SECTION CONTROLS, KERNEL=CUBIC
SECTION CONTROLS, KERNEL=QUADRATIC
SECTION CONTROLS, KERNEL=QUINTIC

Abaqus/CAE Usage

In Abaqus/CAE you can choose the order of the kernel used for interpolation only in Abaqus/Explicit analyses involving the conversion of continuum elements to SPH particles.

Mesh module: MeshElement Type: Conversion to particles: Kernel: Cubic, Quadratic, or Quintic

Using Section Controls for Specifying the SPH Formulation

By default, the SPH kernels satisfy the zero-order completeness requirement. A first-order complete corrected (normalized) kernel is also available, which is sometimes referred in the literature as the normalized SPH (NSPH) method. In high-deformation solid mechanics analyses the use of the NSPH method might lead to more accurate results.

In the SPH methods, a mean velocity filtering coefficient can be used for the modified coordinate updates for particles. A nonzero value for this coefficient leads to the XSPH method, as discussed in Smoothed Particle Hydrodynamics.

Input File Usage

Use one of the following options to specify the SPH formulation:

SECTION CONTROLS, SPH FORMULATION=CLASSICAL (default)
SECTION CONTROLS, SPH FORMULATION=NSPH
SECTION CONTROLS, SPH FORMULATION=XSPH

Abaqus/CAE Usage

In Abaqus/CAE you can only specify section controls for SPH parameters in Abaqus/Explicit analyses involving the conversion of continuum elements to SPH particles.

Using Section Controls for Specifying SPH Parameters

You can control the way the smoothing length is computed (see Smoothed Particle Hydrodynamics). You can specify the smoothing length (units of length) for precise control of the radius of influence associated with a given particle. Alternatively, you can scale the default smoothing length by specifying a dimensionless smoothing length factor. By default, the smoothing length is kept constant throughout the analysis. You can specify a variable smoothing length that increases or decreases during the analysis depending on the divergence of the velocity field, which is a measure of compressive or expansive behavior.

You can also specify the minimum number of particles within the sphere of influence for the given particle. If the total number of particles within the sphere of influence for the given particle is less than the specified minimum number of particles, the deformation gradient for this given particle is frozen, that is, unchanged between the previous and current time increment. In solid mechanics it means that the strain associated with this element will not be changed during the current time increment.

You can specify a mean velocity filtering coefficient that is used for the modified coordinate updates for particles using the XSPH method.

Input File Usage

Use the following option to specify SPH parameters:

SECTION CONTROLS 
first data line
smoothing length, smoothing length factor,
min number of neighboring particles, , mean velocity filtering coefficient

Use one of the following options to define the smoothing length:

SECTION CONTROLS, SPH SMOOTHING LENGTH=CONSTANT (default)
SECTION CONTROLS, SPH SMOOTHING LENGTH=VARIABLE

Abaqus/CAE Usage

In Abaqus/CAE you can only specify section controls for SPH parameters in Abaqus/Explicit analyses involving the conversion of continuum elements to SPH particles.

Using Section Controls to Convert Continuum Elements to Particles

Reduced-integration continuum elements can convert to particles if a certain criterion is met, as discussed in Finite Element Conversion to SPH Particles. You can specify the number of particles per parent element to be generated. Several criteria to trigger the conversion are available.

Input File Usage

Use the following option to prevent finite elements from converting to particles:

SECTION CONTROLS, ELEMENT CONVERSION=NO (default)

Use the following option to trigger the conversion of finite elements to particles based on a uniform background grid:

SECTION CONTROLS, ELEMENT CONVERSION=YES, SPH CONVERSION=BACKGROUND GRID (default)

Use the following option to trigger the conversion of finite elements to particles based on per element conversion:

SECTION CONTROLS, ELEMENT CONVERSION=YES, SPH CONVERSION=PER ELEMENT

Abaqus/CAE Usage

Mesh module: MeshElement Type: Conversion to particles: No or Yes

Generating particles based on a uniform background grid is not supported in Abaqus/CAE.

Specifying the Number of Particles Generated

You specify the number of particles to be generated per isoparametric direction. The number of particles can range from 1 to 7.

Input File Usage

SECTION CONTROLS, ELEMENT CONVERSION=YES, SPH CONVERSION=PER ELEMENT
first data line
second data line
third data line
number of particles to be generated per isoparametric direction

Abaqus/CAE Usage

Mesh module: MeshElement Type: Conversion to particles: Yes, PPD: number of particles to be generated per isoparametric direction

Specifying the Background Grid

You specify the spacing of the background grid and the name of an orientation definition to define a local coordinate system for the background grid.

Input File Usage

SECTION CONTROLS, ELEMENT CONVERSION=YES, SPH CONVERSION=BACKGROUND GRID (default)
first data line
second data line
third data line
spacing of the background grid, name of an orientation definition

Abaqus/CAE Usage

Generating particles based on a uniform background grid is not supported in Abaqus/CAE.

Specifying the Thickness of Generated Particles

The thickness of the particles is primarily used in resolving initial overclosures between the particles and the surfaces in the general contact. When particles are generated based on the uniform background method, you can specify the thickness of the generated particles to be either variable or uniform.

Input File Usage

Use one of the following options to define the thickness of the generated particles:

SECTION CONTROLS, PARTICLE THICKNESS=VARIABLE (default)
SECTION CONTROLS, PARTICLE THICKNESS=UNIFORM

Abaqus/CAE Usage

Generating particles based on a uniform background grid is not supported in Abaqus/CAE.

Specifying a Time-Based Criterion

The time-based criterion is primarily intended as a modeling tool to allow all particles to convert from the defined finite element mesh at the same time.

Input File Usage

SECTION CONTROLS, ELEMENT CONVERSION=YES, SPH CONVERSION=PER ELEMENT
CONVERSION CRITERION=TIME (default) 
first data line
second data line
third data line
 , time of conversion

Abaqus/CAE Usage

Mesh module: MeshElement Type: Conversion to particles: Yes, Criterion: Time

Specifying a Strain-Based Criterion

The strain-based criterion is primarily intended for cases in which you want to use a progressive conversion approach. You specify the maximum principle strain (absolute value) when continuum elements are to convert to SPH particles.

Input File Usage

SECTION CONTROLS, ELEMENT CONVERSION=YES, SPH CONVERSION=PER ELEMENT
CONVERSION CRITERION=STRAIN
first data line
second data line
third data line
 , maximum principle strain (absolute value)

Abaqus/CAE Usage

Mesh module: MeshElement Type: Conversion to particles: Yes, Criterion: Strain

Specifying a Stress-Based Criterion

Similar to the strain-based criterion, the stress-based criterion is primarily intended for cases in which you want to use a progressive conversion approach. You specify the maximum principle stress (absolute value) when continuum elements are to convert to SPH particles.

Input File Usage

SECTION CONTROLS, ELEMENT CONVERSION=YES, SPH CONVERSION=PER ELEMENT
CONVERSION CRITERION=STRESS
first data line
second data line
third data line
 , maximum principle stress (absolute value)

Abaqus/CAE Usage

Mesh module: MeshElement Type: Conversion to particles: Yes, Criterion: Stress

Specifying a User Subroutine–Based Criterion

The user subroutine–based criterion allows you to implement a user-defined conversion criterion. You can control element conversion during the course of an Abaqus/Explicit analysis through any of the user subroutines that can actively modify state variables associated with a material point, such as VUSDFLD and VUMAT.

Input File Usage

Use the following option to trigger a user subroutine–based conversion criterion:

SECTION CONTROLS, CONVERSION CRITERION=USER, ELEMENT CONVERSION=YES, SPH CONVERSION=PER ELEMENT

Abaqus/CAE Usage

Specifying a user subroutine–based criterion for element conversion is not supported in Abaqus/CAE.