Writing Element Output to the Output Database

You can request that element variables (stresses, strains, section forces, element energies, etc.) be written to the output database.

This page discusses:

The output request can be repeated as often as necessary to define output for different types of element variables, different element sets, etc. The same element (or element set) can appear in several output requests. Element output to the output database is not supported for user elements.

 

See Also
About Output
*OUTPUT

Selecting the Element Output Variables

The following types of element variables are recognized for the purpose of defining output:

  • Element integration point variables are associated with the integration points at which material calculations are performed (for example, components of stress and strain).

  • Element section point variables are associated with the cross-section of a beam, pipe, or a shell (for example, bending moments and membrane forces on the section).

  • Element face variables are associated with the faces of a shell or a solid (for example, uniformly distributed pressure load on the face).

  • Whole element variables are attributes of an entire element (for example, the total energy content of the element).

  • Whole element set variables are attributes of an entire element set (for example, the current coordinates of the center of mass); these variables are available in Abaqus/Standard and Abaqus/Explicit.

Selecting Elements for Which Output Is Required

For history output you must specify the element set (or, in Abaqus/Explicit, the tracer set) for which output is being requested. For field output specifying the element set or tracer set is optional; if you do not specify an element set or tracer set, the output will be written for all the elements in the model.

Requesting Field Output for the Exterior Elements in the Model

You can select output on the element set consisting of all the exterior three-dimensional elements in the model. This element set is generated internally by Abaqus.

Specifying the Section Point in Beam, Pipe, Shell, and Layered Solid Elements

For beams, pipes, shells, or layered solids output is provided at the default section points. You can specify nondefault output points.

Requesting Output at All Section Points in Beam, Pipe, Shell, and Layered Solid Elements

You can specify that output be provided for all section points in beams, pipes, shells, and layered solids.

Requesting Output for Rebars in a Reinforced Model

You can request output for rebars (Defining Reinforcement). If you do not explicitly request rebar output in a model with rebars, the element output requests govern the output for the matrix material only (except for section forces, where the forces in the rebar are included in the force calculation). You can request output for a particular rebar. If you do not specify the name of a rebar, output will be given for all rebars in the specified element set (or in the whole model, if you have not specified an element set).

Rebar output is available only in membrane, shell, or surface elements at the integration points and at the centroid of the element.

Selecting the Position of Element Integration Point and Section Point Output

Integration point variables and section variables in Abaqus/Standard can be written as field output to the output database in four different positions: the integration points, the centroid, averaged at nodes, or extrapolated to the nodes. Integration point variables and section variables in Abaqus/Explicit can be written as field output to the output database in three different positions: the integration points, the centroid, or the nodes. By default, output is provided at the integration points.

In most cases Abaqus/Explicit writes only integration point data to the output database. Transferring of results from the integration points to the user-specified position in Abaqus/Explicit is done by the postprocessing calculator. See The Postprocessing Calculator for details.

Element history output to the output database is always provided at the integration points.

Obtaining Output at the Integration Points

By default, the variables are output at the integration points where they are calculated. In Abaqus/Standard you can obtain the position of the integration points by using output variable COORD.

Obtaining Output at the Centroid of Each Element

You can choose to output the variables at the centroid of each element (the midpoint between the end nodes of a beam or a pipe element). Centroidal values are obtained by interpolation of the integration point values if the integration scheme for the element does not include a centroidal integration point. Element output of the element centroidal values is not available for recovering results within substructures; for more information, see Using Substructures.

Obtaining Element Output Extrapolated to the Nodes

You can choose to extrapolate the element integration point variables to the nodes of each element independently, without averaging the results from adjoining elements. Element output at the element nodes is not available for recovering results within substructures; for more information, see Using Substructures.

Obtaining Element Output Averaged at the Nodes in Abaqus/Standard

You can choose to extrapolate the variables to the nodes and to then average them over all of the elements in the set that contribute to each node. For derived variables, such as stress invariants, Abaqus/Standard first averages the extrapolated tensor components over all of the elements connected to the node to obtain unique components at each node and then calculates the derived value based on the averaged components.

By default, Abaqus/Standard partitions the elements in the model into averaging regions. The partitioning is based upon the structure of the elements: element type, number of section points, type of material, single layer or composite, etc. Partitioning is not based upon the values of element properties (such as thickness), material orientations, or material constants. Averaging occurs only over elements that contribute to a node and belong to the same averaging region.

In some situations you may want the averaging regions to take into account the values of element properties. For example, since variables may be discontinuous between elements with different material constants, you may not want elements with different property definitions included in the same averaging region. In such cases you can force Abaqus/Standard to take into account values of element properties by setting the Abaqus environment parameter average_by_section to ON. However, in problems with many section and/or material definitions the default value of OFF will, in general, give much better performance than the nondefault value of ON.

Extrapolation and Interpolation of Element Output Variables

The shape functions of the element are used for purposes of extrapolation and interpolation of output variables. Extrapolated values are generally not as accurate as the values calculated at the integration points in the areas of high stress gradients, particularly in the case of modified triangles and tetrahedra. Therefore, adequately detailed meshing is necessary around nodes where accurate nodal values of such element results are needed. If a cylindrical or spherical coordinate system is defined for the element (see Orientations), the orientation at each integration point may be different. When the values at the integration points are extrapolated to the nodes, the difference in the orientation is not taken into account; therefore, if the orientation varies significantly over the elements connected to a node, the extrapolated values are not very accurate. If the material orientation undergoes significant spatial variation in a region of the model where the material behavior is truly anisotropic, a finer mesh is required to obtain accurate results even at the integration points. In that situation once the overall solution has converged with respect to the mesh density, the interpolation or extrapolation away from the integration points can also be assumed to be reasonably accurate. You should also be particularly careful when interpreting output variables extrapolated to the nodes for second-order elements with midside nodes outside the quarter-point region, such as when one edge is collapsed in two dimensions or one face is collapsed in three dimensions.

For derived variables, such as Mises equivalent stress, the components are first extrapolated or interpolated. The derived value is then calculated from the extrapolated or interpolated components. However, in linear mode-based dynamic analysis procedures where derived values are obtained as nonlinear combinations of modal response magnitudes (Random Response Analysis and Response Spectrum Analysis), the nonlinear combinations are first calculated at the integration points. These derived values are then extrapolated to the nodes or interpolated to the centroid.

Requesting Preselected Output

You can request the preselected, procedure-specific element output variables described in Preselected Output Requests. In this case you can specify additional variables as part of the output request.

Alternatively, you can request all element variables applicable to the current procedure and material type. In this case any additional variables you specify are ignored.

Specifying the Directions for Element Output

For components of stress, strain, and similar material variables 1, 2, and 3 refer to the directions for an orthogonal coordinate system. If a local orientation is not defined for the element, the stress/strain components are in the default directions defined by the convention given in Orientations: global directions for solid elements, surface directions for shell and membrane elements, and axial and transverse directions for beam and pipe elements.

By default, the element material directions for element field output are written to the output database. You can choose to suppress the direction output to the output database.