MultiPhysicsVault/.raw/AbaqusAnalysisUserGuide1/AbaqusAnalysisUserGuide1_072.md

finite-membrane-strain shell elements, membrane elements, and continuum elements associated with a local orientation (see “Orientations,” Section 2.2.5), the local output directions rotate with the average rotation of the element (integral with respect to time of the spin—see “Stress rates,” Section 1.5.3 of the Abaqus Theory Guide). Tensor components in these cases are output in the rotating local directions.

In some cases the local output directions may differ from one integration point to the next within an element. Abaqus/Standard does not take this variation into account when extrapolating output variables to the nodes, which affects output such as element quantities averaged at the nodes or contour plots of individual tensor components. Invariant quantities at the integration points will not be influenced by the local output directions.

You can control writing the local directions to the output database file or to the results file (see “Specifying the directions for element output in Abaqus/Standard and Abaqus/Explicit” in “Output to the output database,” Section 4.1.3, and “Output of local directions to the results file” in “Output to the data and results files,” Section 4.1.2). By default, the local directions are written to the output database for all frames that include element field output. The local (material) directions (averaged at the nodes) can be visualized in Abaqus/CAE by selecting Plot→Material Orientations in the Visualization module. The directions can be printed to the data file by using user subroutine UVARM.

Direction definitions for equivalent rigid body variables

For all equivalent rigid body variables 1, 2, and 3 refer to global directions.

Direction definitions for nodal variables

For nodal variables 1, 2, and 3 are global directions (1=X, 2=Y, and 3=Z; or for axisymmetric elements, 1=r and 2=z). If a local coordinate system is defined at a node (see “Transformed coordinate systems,” Section 2.1.5), you can specify whether output to the data or results file of vector-valued quantities at these nodes is in the local or global system (see “Specifying the directions for nodal output” in “Output to the data and results files,” Section 4.1.2). By default, nodal output is written to the data file in the local system, whereas it is written to the results file in the global system (since this is more convenient for postprocessing).

If nodal field output is requested for a node that has a local coordinate system defined, a quaternion representing the rotation from the global directions is written to the output database. Abaqus/CAE automatically uses this quaternion to transform the nodal results into the local directions. Nodal history data written to the output database are always stored in the global directions.

Direction definitions for integrated variables

For components of total force, total moment, and similar variables obtained through integration over a surface, the directions 1, 2, and 3 refer to directions in an orthogonal coordinate system. A fixed global coordinate system is used if the surface is specified directly for the integrated output request. If the surface is identified by an integrated output section definition (see “Integrated output section definition,” Section 2.5.1) that is associated with the integrated output request, a local coordinate system in the initial configuration can be specified and can translate or rotate with the deformation.

Distributed load output

You need to be aware of limitations that may be encountered when distributed load output is requested.

Distributed load output and user subroutines

Output can be requested for many of the distributed loads discussed in “Loads,” Section 34.4. However, contributions to these loads defined through user subroutines (see “Abaqus/Standard subroutines,” Section 1.1 of the Abaqus User Subroutines Reference Guide) are not displayed, except for the variables FILMCOEF and SINKTEMP.

Distributed load output with modal procedures

For modal procedures only the magnitude of the load is written to the output database.

Strain output

The total strain E is composed of the elastic strain EE, the inelastic strain IE, and the thermal strain THE. The inelastic strain IE consists of the plastic strain PE and the creep strain CE.

For geometrically nonlinear analysis Abaqus/Standard makes it possible to output different strain measures as well as elastic and various inelastic strains. The various total strain measures (integrated strain measure E, nominal strain measure NE, and logarithmic strain measure LE) are described in “Conventions,” Section 1.2.2. The default strain measure for output to the data (.dat) and results (.fil) files is E. However, for geometrically nonlinear analysis using element formulations that support finite strains, E is not available for output to the output database (.odb) file, and LE is the default strain measure.

Temperature output

In Abaqus temperature can either be a field variable (stress analysis, mass diffusion, …) or a degree of freedom (heat transfer analysis, fully coupled temperature-displacement analysis, …). For any analysis that involves temperature, you can request the temperature either at nodes (variable NT) or in elements (variable TEMP). If element temperature output is requested at the nodes, the integration point values are extrapolated and, if requested, averaged. These extrapolated values are generally not as accurate as the nodal temperatures themselves. An exception to this is adiabatic analysis, in which the element temperatures change due to plastic heat generation but the nodal temperatures are not updated. In that case the current nodal temperatures are obtained only if element temperature output is requested at the nodes.

For continuum elements there is only one temperature value per node (NT11). For shells and beams more than one temperature is available for each node (NT11, NT12, …) since a temperature gradient can exist through the thickness of a shell or across the cross-section of a beam. In general, variables NT12, NT13, etc. contain temperature values. However, when temperature is defined by specifying temperature gradients, nodal temperatures for a given section point can be obtained only by using the variable TEMP. See “Specifying temperature and field variables” in “Using a beam section integrated

during the analysis to define the section behavior,” Section 29.3.6, and “Specifying temperature and field variables” in “Using a shell section integrated during the analysis to define the section behavior,” Section 29.6.5, for discussions on specifying temperatures in beams and shells.

Principal value output

Output of the principal values can be requested for stresses, strains, and other material tensors. Either all principal values or the minimum, maximum, or intermediate values can be obtained. All principal values of tensor ABC are obtained with the request ABCP. The minimum, intermediate, and maximum principal values are obtained with the requests ABCP1, ABCP2, and ABCP3.

For three-dimensional, (generalized) plane strain, and axisymmetric elements all three principal values are obtained. For plane stress, membrane, and shell elements, the out-of-plane principal value cannot be requested for history-type output. For field-type output, Abaqus/CAE always reports the outof-plane principal value as zero. Principal values cannot be obtained for truss elements or for any beam elements other than the three-dimensional beam elements with torsional shear stresses.

If a principal value or an invariant is requested for field-type output, the output request is replaced with an output request for the components of the corresponding tensor. Abaqus/CAE calculates all principal values and invariants from these components. If a principal value is desired as history-type output, it must be explicitly requested since Abaqus/CAE does no calculations on history data.

Tensor output

Tensor variables that are written to the output database as field-type output are written as components in either the default directions defined by the convention given in “Orientations,” Section 2.2.5 (global directions for solid elements, surface directions for shell and membrane elements, and axial and transverse directions for beam elements), or the user-defined local system. Abaqus/CAE calculates all principal values and invariants from these components. See “Writing field output data,” Section 9.6.4 of the Abaqus Scripting User’s Guide, for a description of the different types of tensor variables.

For plane stress, membrane, and shell elements, only the in-plane tensor components (11, 22, and 12 components) are stored by Abaqus/Standard. The out-of-plane direct component for stress (S33) is reported as zero to the output database as expected, and the out-of-plane component of strain (E33) is reported as zero even though it is not. This is because the thickness direction is computed based on section properties rather than at the material level. The out-of-plane components can be requested for field-type output and cannot be requested for history-type output. The out-of-plane stress components are not reported to the data (.dat) file or to the results (.fil) file.

For three-dimensional beam elements with torsional shear stresses, only the axial and the torsional components (the 11 and 12 components) are stored by Abaqus/Standard. The other direct component (the 22 component) is reported as zero for field-type output and cannot be requested for history-type output.

The components for tensor variables are written to the output database in single precision. Therefore, a small amount of precision roundoff error may occur when calculating the variables’ principal values. Such roundoff error may be observed, for example, when analytically zero values are calculated as relatively small nonzero values.

Element integration point variables

You can request element integration point variable output to the data, results, or output database file (see “Element output” in “Output to the data and results files,” Section 4.1.2, and “Element output” in “Output to the output database,” Section 4.1.3).

Identifier	.dat	.fil	.odb	Description
			Field History

Tensors and associated principal values and invariants

S	●	●	●	●	All stress components.
Sij	●			●	ij-component of stress (i ≤ j ≤ 3).
SP	●	●	●	●	All principal stresses.
SPn	●			●	Minimum, intermediate, and maximum principal stresses (SP1 ≤ SP2 ≤ SP3).
SINV	●	●	●	●	All stress invariant components (MISES, TRESC, PRESS, INV3). For field output SINV is converted to a request for the generic variable S.
MISES	●			●	Mises equivalent stress, defined as

$$ q = \sqrt {\frac {3}{2} \mathbf {S} : \mathbf {S}}, $$

where is the deviatoric stress tensor, defined as \mathbf { S } = { \boldsymbol { \sigma } } + p \mathbf { I } where \sigma is the stress, p is the equivalent pressure stress (defined below), and is a unit matrix. In index notation

q = \sqrt {\frac {3}{2} S _ {i j} S _ {i j}},

where \begin{array} { r } { S _ { i j } = \sigma _ { i j } + p \delta _ { i j } , p = - \frac { 1 } { 3 } \sigma _ { i i } } \end{array} , and \delta _ { i j } is the Kronecker delta.

MISESMAX	Maximum Mises stress among all of the section points. For a shell element it represents the maximum Mises value among all the section points in the layer, for a beam element it is the maximum Mises stress among all the section points in the cross-section, and for a solid element it represents the Mises stress at the integration points.
MISESONLY	Mises equivalent stress. When MISESONLY is used instead of MISES, the stress components are not written to the output database; consequently, the size of the database is reduced.

Identifier	.dat	.fil	.odb		Description
			Field	History
TRESC	•			•	Tresca equivalent stress, defined as the maximum difference between principal stresses.
PRESS	•			•	Equivalent pressure stress, defined as $p = -\frac{1}{3}\text{trace}(\sigma) = -\frac{1}{3}\sigma_{ii}$ .
PRESSONLY			•		Equivalent pressure stress. When PRESSONLY is used instead of PRESS, the stress components are not written to the output database; consequently, the size of the database is reduced.
INV3	•			•	Third stress invariant, defined as $r = \left(\frac{9}{2}\mathbf{S} \cdot \mathbf{S} : \mathbf{S}\right)^{1/3} = \left(\frac{9}{2}S_{ij}S_{jk}S_{ki}\right)^{1/3}$ , where S is the deviatoric stress defined in the context of Mises equivalent stress, above.
TRIAX			•	•	Stress triaxiality, $\eta = -p/q$ .
YIELDS			•	•	Yield stress, $\sigma^0$ , available for Mises, Johnson-Cook, and Hill plasticity material models.
ALPHA	•	•	•	•	All total kinematic hardening shift tensor components.
ALPHAij	•			•	ij-component of the total shift tensor ( $i \leq j \leq 3$ ).
ALPHAk			•	•	All $k^{th}$ kinematic hardening shift tensor components ( $1 \leq k \leq 10$ ).
ALPHAk_ij				•	ij-component of the $k^{th}$ kinematic hardening shift tensor ( $i \leq j \leq 3$ and $1 \leq k \leq 10$ ).
ALPHAN			•	•	All tensor components of all the kinematic hardening shift tensors, except the total shift tensor, ALPHA.
ALPHAP	•	•	•	•	All principal values of the total shift tensor.
ALPHAPn	•			•	Minimum, intermediate, and maximum principal values of the total shift tensor (ALPHAP1 $\leq$ ALPHAP2 $\leq$ ALPHAP3).
SNETk			•	•	All stress components in the $k^{th}$ network ( $0 \leq k \leq 10$ ). Available only for the parallel rheological framework.
SNETk_ij				•	ij-component of stress in the $k^{th}$ network ( $i \leq j \leq 3$ and $0 \leq k \leq 10$ ). Available only for the parallel rheological framework.

Identifier	.dat	.fil	.odb		Description
			Field	History
E	•	•	•	•	All strain components. For geometrically nonlinear analysis using element formulations that support finite strains, E is not available for output to the output database (.odb) file.
Eij	•			•	ij-component of strain (i ≤ j ≤ 3).
EP	•	•	•	•	All principal strains.
EPn	•			•	Minimum, intermediate, and maximum principal strains (EP1 ≤ EP2 ≤ EP3).
NE	•	•	•	•	All nominal strain components.
NEij	•			•	ij-component of nominal strain (i ≤ j ≤ 3).
NEP	•	•	•	•	All principal nominal strains.
NEPn	•			•	Minimum, intermediate, and maximum principal nominal strains (NEP1 ≤ NEP2 ≤ NEP3).
LE	•	•	•	•	All logarithmic strain components. For geometrically nonlinear analysis using element formulations that support finite strains, LE is the default strain measure for output to the output database (.odb) file.
LEij	•			•	ij-component of logarithmic strain (i ≤ j ≤ 3).
LEP	•	•	•	•	All principal logarithmic strains.
LEPn	•			•	Minimum, intermediate, and maximum principal logarithmic strains (LEP1 ≤ LEP2 ≤ LEP3).
ER	•	•	•	•	All mechanical strain rate components.
ERij	•			•	ij-component of strain rate (i ≤ j ≤ 3).
ERP	•	•	•	•	All principal mechanical strain rates.
ERPn	•			•	Minimum, intermediate, and maximum principal mechanical strain rates (ERP1 ≤ ERP2 ≤ ERP3).
DG	•	•			All components of the total deformation gradient. Available only for hyperelasticity, hyperfoam, and material models defined in user subroutine UMAT. For fully integrated first-order quadrilaterals and hexahedra, the selectively reduced integration technique is used. A modified deformation gradient is output for these elements.
DGij	•				ij-component of the total deformation gradient (i, j ≤ 3).
DGP	•	•			Principal stretches.

Identifier	.dat	.fil	.odb		Description
			Field	History
DGPn	•				Minimum, intermediate, and maximum values of principal stretches (DGP1 ≤ DGP2 ≤ DGP3).
EE	•	•	•	•	All elastic strain components.
EEij	•			•	ij-component of elastic strain (i ≤ j ≤ 3).
EEP	•	•	•	•	All principal elastic strains.
EEPn	•			•	Minimum, intermediate, and maximum principal elastic strains (EEP1 ≤ EEP2 ≤ EEP3).
IE	•	•	•	•	All inelastic strain components.
IEij	•			•	ij-component of inelastic strain (i ≤ j ≤ 3).
IEP	•	•	•	•	All principal inelastic strains.
IEPn	•			•	Minimum, intermediate, and maximum principal inelastic strains (IEP1 ≤ IEP2 ≤ IEP3).
THE	•	•	•	•	All thermal strain components.
THEij	•			•	ij-component of thermal strain (i ≤ j ≤ 3).
THEP	•	•	•	•	All principal thermal strains.
THEPn	•			•	Minimum, intermediate, and maximum principal thermal strains (THEP1 ≤ THEP2 ≤ THEP3).
PE	•	•	•	•	All plastic strain components. This identifier also provides PEEQ, a yes/no flag telling if the material is currently yielding or not (AC YIELD: “actively yielding”; that is, the plastic strain changed during the increment), and PEMAG when PE is requested for the data or results files. When PE is requested for field output to the output database, PEEQ is also provided.
PEij	•			•	ij-component of plastic strain (i ≤ j ≤ 3).
PEEQ	•		•	•	Equivalent plastic strain. This identifier also provides

\int _ { 0 } ^ { t } \dot { \bar { \varepsilon } } ^ { p l } \dot { d t } ivalent, where \bar { \varepsilon } ^ { p l } | _ { 0 } ic strain is defined asis the initial equivalen \bar { \varepsilon } ^ { p l } | _ { 0 } + strain.

The definition of \dot { \bar { \varepsilon } } ^ { p l } depends on the material model. For classical metal (Mises) plasticity

Identifier	.dat	.fil	.odb		Description
			Field	History
					$\dot{\varepsilon}^{pl} = \sqrt{\frac{2}{3} \dot{\varepsilon}^{pl} : \dot{\varepsilon}^{pl}}$ . For other plasticity models, see the appropriate section in Part V, “Materials.”
					When plasticity occurs in the thickness direction to a gasket element whose plastic behavior is specified as part of a gasket behavior definition, PEEQ is PE11.
PEEQMAX			•		Maximum equivalent plastic strain, PEEQ, among all of the section points. For a shell element it represents the maximum PEEQ value among all the section points in the layer, for a beam element it is the maximum PEEQ among all the section points in the cross-section, and for a solid element it represents the PEEQ at the integration points.
PEEQT	•	•	•	•	Equivalent plastic strain in uniaxial tension for cast iron, Mohr-Coulomb tension cutoff, and concrete damaged plasticity, which is defined as $\int \dot{\varepsilon}_{t}^{pl} dt$ . This identifier also provides a yes/no flag (1/0 on the output database) telling if the material is currently yielding or not (AC YIELDT: “actively yielding”; that is, the plastic strain changed during the increment).
PEMAG	•		•	•	Plastic strain magnitude, defined as $\sqrt{\frac{2}{3} \varepsilon^{pl} : \varepsilon^{pl}}$ .
					For most materials, PEEQ and PEMAG are equal only for proportional loading. When plasticity occurs in the thickness direction to a gasket element whose plastic behavior is specified as part of a gasket behavior definition, PEMAG is PE11.
PEP	•	•	•	•	All principal plastic strains.
PEPn	•			•	Minimum, intermediate, and maximum principal plastic strains (PEP1 ≤ PEP2 ≤ PEP3).
CE	•	•	•	•	All creep strain components. This identifier also provides CEEQ, CESW, and CEMAG when CE is requested for the data or results files.
CEij	•			•	ij-component of creep strain (i ≤ j ≤ 3).
CEEQ	•		•	•	Equivalent creep strain, defined as $\int_{0}^{t} \dot{\varepsilon}^{cr} dt$ .
					The definition of $\dot{\varepsilon}^{cr}$ depends on the material model. For classical metal (Mises) creep $\dot{\varepsilon}^{cr} = \sqrt{\frac{2}{3} \dot{\varepsilon}^{cr} : \dot{\varepsilon}^{cr}}$ .

Identifier	.dat	.fil	.odb		Description
			Field	History
					For other creep models, see the appropriate section in Part V, “Materials.”
					When creep occurs in the thickness direction to a gasket element whose creep behavior is specified as part of a gasket behavior definition, CEEQ is CE11.
CESW	•		•	•	Magnitude of swelling strain.
					For cap creep CESW gives the equivalent creep strain produced by the consolidation creep mechanism, defined as $\int \frac{\sigma: d\varepsilon^{cr}}{\bar{p}}$ , where $\bar{p}$ is the equivalent creep pressure, $\bar{p} = (R^2 q^2 + p (p - p_a)) / G_c^{cr}$ .
CEMAG	•		•	•	Magnitude of creep strain (defined by the same formula given above for PEMAG, applied to the creep strains).
CEP	•	•	•	•	All principal creep strains.
CEPn	•			•	Minimum, intermediate, and maximum principal creep strains (CEP1 ≤ CEP2 ≤ CEP3).
Additional element stresses
CS11	•	•	•	•	Average contact pressure for link and three-dimensional line gasket elements. Available only if the gasket contact area is specified; see “Defining the contact area for average contact pressure output” in “Defining the gasket behavior directly using a gasket behavior model,” Section 32.6.6.
TSHR	•	•	•	•	All transverse shear stress components. Available only for thick shell elements such as S3R, S4R, S8R, and S8RT. Contouring of this variable is supported in the Visualization module of Abaqus/CAE.
TSHRi3	•			•	i3-component of transverse shear stress (i = 1, 2). Available only for thick shell elements such as S3R, S4R, S8R, and S8RT.
CTSHR	•		•	•	Transverse shear stress components for stacked continuum shell elements. Available only for SC6R and SC8R elements. Contouring of this variable is supported in the Visualization module of Abaqus/CAE.

Identifier	.dat	.fil	.odb		Description
			Field	History
CTSHRi3	•			•	i3-component of transverse shear stress (i = 1,2). Available only for SC6R and SC8R elements.
SS	•	•			All substresses. Available only for ITS elements.
SSn	•				nth substress (n = 1,2). Available only for ITS elements.

Vibration and acoustic quantities

INTEN	•	•	Vibration intensity. Available only for the steady-state dynamics procedure. For real-only steady-state dynamics analyses, the intensity is a pure imaginary vector, but it is stored as real on the output database. Available for structural, solid, and acoustic elements and for rebar.
ACV	•	•	Acoustic particle velocity. Available only if the steady-state dynamic procedure is used, and available only for acoustic finite elements.
ACVn		•	Component n of the acoustic particle velocity vector (n = 1, 2, 3). Available only if the steady-state dynamic procedure is used, and available only for acoustic finite elements.
GRADP	•	•	Acoustic pressure gradient. Available only if the steady-state dynamic procedure is used, and available only for acoustic finite elements.

Energy densities

In steady-state dynamics all energy quantities are net per-cycle values, unless otherwise noted (see “Energy balance,” Section 1.5.5 of the Abaqus Theory Guide).

ENER	•	•	•	•	All energy densities. None of the energy densities are available in mode-based procedures; a limited number of them are available for direct-solution steady-state dynamic and subspace-based steady-state dynamic analyses.
SENER	•		•	•	Elastic strain energy density (with respect to current