<!-- source-page: 61 -->

# Analysis types

The Joule heating effect requires full coupling of the thermal and electrical problems (see “Coupled thermal-electrical analysis,” Section 6.7.3). The coupling arises from two sources: temperature-dependent electrical conductivity and the heat generated in the thermal problem by electric conduction.

These elements can also be used to perform uncoupled electric conduction analysis in all or part of the model. In such analysis only the electric potential degree of freedom is activated, and all heat transfer effects are ignored. This capability is available by omitting the thermal conductivity from the material definition.

The coupled thermal-electrical elements can also be used in heat transfer analysis (“Uncoupled heat transfer analysis,” Section 6.5.2), in which case all electric conduction effects are ignored. This feature is quite useful if a coupled thermal-electrical analysis is followed by a pure heat conduction analysis (such as a welding simulation followed by cool down).

The elements cannot be used in any of the stress/displacement analysis procedures.

# Active degrees of freedom

Coupled thermal-electrical elements have both temperature and electrical potential degrees of freedom. See “Conventions,” Section 1.2.2, for a discussion of the degrees of freedom in Abaqus.

# Interpolation

Coupled thermal-electrical elements are provided with first- or second-order interpolation of the temperature and electrical potential.

# Choosing a coupled thermal-electrical element

Coupled thermal-electrical elements are available only in the following element family:

• “Solid (continuum) elements,” Section 28.1.1.

# Piezoelectric elements

Piezoelectric elements are provided in Abaqus/Standard for problems in which a coupling between the stress and electrical potential (the piezoelectric effect) must be modeled.

# Analysis types

Piezoelectric elements are for use in piezoelectric analysis (“Piezoelectric analysis,” Section 6.7.2).

# Active degrees of freedom

The piezoelectric elements have both displacement and electric potential degrees of freedom. See “Conventions,” Section 1.2.2, for a discussion of the degrees of freedom in Abaqus. The piezoelectric effect is discussed further in “Piezoelectric analysis,” Section 6.7.2.

<!-- source-page: 62 -->

# Interpolation

Piezoelectric elements are available with first- or second-order interpolation of displacement and electrical potential.

# Choosing a piezoelectric element

Piezoelectric elements are available in the following element families:

• “Solid (continuum) elements,” Section 28.1.1; and   
• “Truss elements,” Section 29.2.1.

# Electromagnetic elements

Electromagnetic elements are provided in Abaqus/Standard for problems that require the computation of the magnetic fields (such as a magnetostatic analysis) or for problems in which a coupling between electric and magnetic fields must be modeled (such as an eddy current analysis).

# Analysis types

Electromagnetic elements are for use in magnetostatic and eddy current analyses (“Magnetostatic analysis,” Section 6.7.6, and “Eddy current analysis,” Section 6.7.5).

# Active degrees of freedom

Electromagnetic elements have magnetic vector potential as the degree of freedom. See “Conventions,” Section 1.2.2, for a discussion of the degrees of freedom in Abaqus. Magnetostatic analysis is discussed further in “Magnetostatic analysis,” Section 6.7.6, while the electromagnetic coupling that occurs in an eddy current analysis is discussed further in “Eddy current analysis,” Section 6.7.5.

# Interpolation

Electromagnetic elements are available with zero-order element edge–based interpolation of the magnetic vector potential.

# Choosing an electromagnetic element

Electromagnetic elements are available in the following element family:

• “Solid (continuum) elements,” Section 28.1.1.

# Acoustic elements

Acoustic elements are used for modeling an acoustic medium undergoing small pressure changes. The solution in the acoustic medium is defined by a single pressure variable. Impedance boundary conditions representing absorbing surfaces or radiation to an infinite exterior are available on the surfaces of these acoustic elements.

<!-- source-page: 63 -->

Acoustic infinite elements, which improve the accuracy of analyses involving exterior domains, and acoustic-structural interface elements, which couple an acoustic medium to a structural model, are also provided.

# Analysis types

Acoustic elements are for use in acoustic and coupled acoustic-structural analysis (“Acoustic, shock, and coupled acoustic-structural analysis,” Section 6.10.1).

# Active degrees of freedom

Acoustic elements have acoustic pressure as a degree of freedom. Coupled acoustic-structural elements also have displacement degrees of freedom. See “Conventions,” Section 1.2.2, for a discussion of the degrees of freedom in Abaqus.

# Choosing an acoustic element

Acoustic elements are available in the following element families:

• “Solid (continuum) elements,” Section 28.1.1;   
• “Infinite elements,” Section 28.3.1; and   
• “Acoustic interface elements,” Section 32.13.1.

The acoustic elements can be used alone but are often used with a structural model in a coupled analysis. “Acoustic interface elements,” Section 32.13.1, describes interface elements that allow this acoustic pressure field to be coupled to the displacements of the surface of the structure. Acoustic elements can also interact with solid elements through the use of surface-based tie constraints; see “Acoustic, shock, and coupled acoustic-structural analysis,” Section 6.10.1.

# Using the same mesh with different analysis or element types

You may want to use the same mesh with different analysis or element types. This may occur, for example, if both stress and heat transfer analyses are intended for a particular geometry or if the effect of using either reduced- or full-integration elements is being investigated. Care should be taken when doing this since unexpected error messages may result for one of the two element types if the mesh is distorted. For example, a stress analysis with C3D10 elements may run successfully, but a heat transfer analysis using the same mesh with DC3D10 elements may terminate during the datacheck portion of the analysis with an error message stating that the elements are excessively distorted or have negative volumes. This apparent inconsistency is caused by the different integration locations for the different element types. Such problems can be avoided by ensuring that the mesh is not distorted excessively.

<!-- source-page: 64 -->

<!-- source-page: 65 -->

# 27.1.4 SECTION CONTROLS

Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE

# References

• \*SECTION CONTROLS   
• \*HOURGLASS STIFFNESS   
• “Element type assignment,” Section 17.5.3 of the Abaqus/CAE User’s Guide

# Overview

Section controls in Abaqus/Standard:

• choose the hourglass control formulation for most first-order elements with reduced integration;   
• define the distortion control for C3D10HS elements;   
• select the hourglass control scale factors for all elements with reduced integration; and   
• select the choice of element deletion and the value of maximum degradation for cohesive elements, connector elements, elements with plane stress formulations (plane stress, shell, continuum shell, and membrane elements) with constitutive behavior that includes damage evolution, any element that can be used with damage evolution models for ductile metals, and any element that can be used with the damage evolution law in a low-cycle fatigue analysis.

Section controls in Abaqus/Explicit:

• choose the hourglass control formulation or scale factors for all elements with reduced integration;   
• define the distortion control for solid elements;   
• select the scale factors for the drill stiffness of shell elements or deactivate the drill stiffness for small-strain shell elements S3RS and S4RS;   
• select an amplitude for ramping of any initial stresses in membrane elements;   
• select the kinematic formulation for hexahedron solid elements;   
• select the accuracy order of the formulation for solid and shell elements;   
• select the scale factors for linear and quadratic bulk viscosity parameters;   
• specify the size of the particle tracking box for discrete element method (DEM) analyses and smoothed particle hydrodynamic (SPH) analyses;   
• specify the formulation and additional control parameters for SPH analyses; and   
• select the choice of element deletion and the value of maximum degradation for elements with constitutive behavior that includes damage evolution.

In Abaqus/CAE section controls are specified when you assign an element type to particular mesh regions and are referred to as element controls.

<!-- source-page: 66 -->

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. 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 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,” Section 24.1.1; “Connector damage behavior,” Section 31.2.7; and “Defining the constitutive response of cohesive elements using a traction-separation description,” Section 32.5.6). 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

<!-- source-page: 67 -->

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

Abaqus/CAE Usage: Mesh module: Mesh→Element 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 may 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

$$
Q = \int_ {0} ^ {t} s K (t - t ^ {\prime}) \frac {d q}{d t ^ {\prime}} d t ^ {\prime},
$$

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 and membrane elements $s ^ { s }$ scales all hourglass stiffnesses. 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 smallstrain 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. It is the most computationally intensive hourglass control method. It is not supported for Eulerian EC3D8R elements.

Input File Usage: $\ast \mathrm { S E C T I O N ~ C O N T R O L S , ~ N A M E } { = } n a m e ,$ $\mathrm { H O U R G L A S S { = } R E L A X S T I F N E S S }$ $s ^ { s } , s ^ { r } , s ^ { w }$

<!-- source-page: 68 -->

Abaqus/CAE Usage: Mesh module: Mesh→Element 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

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

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

<!-- source-page: 69 -->

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

Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Hourglass control: Combined, Stiffness-viscous weight factor: , 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

$$
Q = s ^ {s} \big ((r _ {F} G) B _ {\alpha} ^ {P} B _ {\alpha} ^ {P} V \big) q,
$$

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; $B _ { \alpha } ^ { P }$ is the gradient interpolator used to define constant gradients in the element $( \partial u / \partial S _ { \alpha } ~ = ~ B _ { \alpha } ^ { P } u ^ { P }$ where the superscript P refers to an element node, the subscript refers to a direction, and $S _ { \alpha }$ 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

$$
Q = s ^ {p} \big ((r _ {F} K) B ^ {P} B ^ {P} V \big) q,
$$

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

<!-- source-page: 70 -->

$$
Q = s ^ {r} \big ((r _ {\theta} G) B _ {\alpha} ^ {P} B _ {\alpha} ^ {P} t ^ {3} A \big) q,
$$

where $s ^ { r }$ is the scale factor (by default, $s ^ { r } = 1 . 0 ) , r _ { \theta } G$ is the hourglass stiffness factor, t is the thickness of the shell element, and A is the area of the shell element.

$\begin{array} { r l } { \mathsf { I n p u t \ F i l e \ U s a g e : } \quad } & { \quad * \mathrm { S E C T I O N \ C O N T R O L S } , \mathrm { N A M E = \# m } e , \mathrm { H O U R G L A S S = S T I F F N E S S } } \\ & { \quad \quad s ^ { s } , s ^ { r } , \ldots , s ^ { p } } \end{array}$

Abaqus/CAE Usage: Mesh module: Mesh→Element 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 may, for example, be given as part of the elastic material definition (“Linear elastic behavior,” Section 22.2.1). 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

$$
G = \frac {1}{3} \left(D _ {1 2 1 2} + D _ {1 3 1 3} + D _ {2 3 2 3}\right)
$$

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

$$
G = \frac {1}{3} (G _ {1 2} + G _ {1 3} + G _ {2 3}).
$$

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

$$
(r _ {F} G) = 0. 0 0 5 G.
$$

For membrane hourglass control in a shell

$$
(r _ {F} G) = 0. 0 0 5 \frac {\int_ {- t / 2} ^ {t / 2} G d t}{t}.
$$

For control of bending hourglass modes in a shell
