<!-- source-page: 671 -->

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,” Section 6.3.11, and “Response spectrum analysis,” Section 6.3.10), the nonlinear combinations are first calculated at the integration points. These derived values are then extrapolated to the nodes or interpolated to the centroid.

# Controlling the output frequency

The frequency of element output is controlled as described above in “Controlling the output frequency.”

# Requesting preselected output

You can request the preselected, procedure-specific element output variables described in Table 4.1.3–1. 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.

<table><tr><td>Input File Usage:</td><td>Use the following option to request the preselected element output variables:*ELEMENT OUTPUT, VARIABLE=PRESELECTUse the following option to request all applicable element output variables:*ELEMENT OUTPUT, VARIABLE=ALL</td></tr></table>

<table><tr><td>Abaqus/CAE Usage:</td><td>Step module: field or history output request editor: Preselected defaults or All</td></tr></table>

# Specifying the directions for element output in Abaqus/Standard and Abaqus/Explicit

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,” Section 2.2.5: 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. If a local orientation is associated with the element, by default the results displayed in Abaqus/CAE are in the directions defined by the local orientation. These directions can be visualized in Abaqus/CAE by selecting Plot→Material Orientations in the Visualization module. You can choose to suppress the direction output to the output database.

<table><tr><td>Input File Usage:</td><td>Use the following option to indicate that the element material directions should not be written to the output database:</td></tr><tr><td></td><td>*ELEMENT OUTPUT, DIRECTIONS=NO</td></tr></table>

<table><tr><td>Abaqus/CAE Usage:</td><td>Step module: field output request editor: toggle off Include local coordinate directions when available</td></tr></table>

<!-- source-page: 672 -->

# Node output

You can output nodal variables (displacements, reaction forces, etc.) to the output database. The output request can be repeated as often as necessary to define output for different node sets. The same node (or node set) can appear in several output requests.

# Selecting the nodal output variables

The nodal variables that can be written to the output database are defined in the “Nodal variables” section of “Abaqus/Standard output variable identifiers,” Section 4.2.1, “Abaqus/Explicit output variable identifiers,” Section 4.2.2, and “Abaqus/CFD output variable identifiers,” Section 4.2.3.

Input File Usage: \*NODE OUTPUT list of output variables

Abaqus/CAE Usage: Step module: field or history output request editor: Select from list below

# Selecting the nodes for which output is required

For history output you must specify the node set (or, in Abaqus/Explicit, the tracer set) for which output is being requested. For field output the specification of the node set or tracer set is optional; if you do not specify a node set or tracer set, the output will be written for all the nodes in the model.

Input File Usage: \*NODE OUTPUT, NSET=node\_set\_name

Abaqus/CAE Usage: Step module: field or history output request editor: Domain: Set: set\_name

Requesting field output for the exterior nodes in the model in Abaqus/Standard and Abaqus/Explicit

You can select output on the node set consisting of all the exterior nodes in the model. This node set is generated internally by Abaqus and includes all the nodes that belong to the exterior three-dimensional elements.

Input File Usage: \*NODE OUTPUT, EXTERIOR

Abaqus/CAE Usage: Step module: field output request editor: Domain: Whole model; toggle on Exterior only

# Controlling the output frequency

The frequency of nodal output is controlled as described above in “Controlling the output frequency.”

# Controlling the precision in Abaqus/Standard and Abaqus/Explicit

You can control the precision of nodal output for an analysis.

Input File Usage: Use the following command line option to request single-precision nodal output:

abaqus job=job-name output\_precision=single

<!-- source-page: 673 -->

Use the following command line option to request double-precision nodal output:

abaqus job=job-name output\_precision=full

Abaqus/CAE Usage: Job module: job editor: Precision: Nodal output precision: Single or Full

# Requesting preselected output

You can request the preselected, procedure-specific nodal output variables described in Table 4.1.3–1. In this case you can specify additional variables as part of the output request.

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

Input File Usage: Use the following option to request the preselected nodal output variables:

\*NODE OUTPUT, VARIABLE=PRESELECT

Use the following option to request all applicable nodal output variables:

\*NODE OUTPUT, VARIABLE=ALL

Abaqus/CAE Usage: Step module: field or history output request editor:

Preselected defaults or All

# Specifying the directions for nodal field output in Abaqus/Standard and Abaqus/Explicit

For nodal variables 1, 2, and 3 refer to the global directions X, Y, and Z, respectively. For axisymmetric elements 1 and 2 refer to the global directions r and z. Nodal field results are written to the output database in the global directions. If a local coordinate system is defined at a node (see “Transformed coordinate systems,” Section 2.1.5), the local nodal transformations are written to the output database as well. You can apply these transformations to the results in the Visualization module of Abaqus/CAE to view components in the local systems.

# Specifying the directions for nodal history output in Abaqus/Standard and Abaqus/Explicit

For nodal variables 1, 2, and 3 refer to the global directions X, Y, and Z, respectively. For axisymmetric elements 1 and 2 refer to the global directions r and z. Nodal history results are written to the output database in the global directions unless a local coordinate system has been defined at a node (see “Transformed coordinate systems,” Section 2.1.5). In this case you can specify whether output is desired in global or local directions.

# Obtaining nodal history output in the global directions

You can request vector-valued nodal variables in the global directions, which is the default for nodal history output requests to the output database since most postprocessors assume that components are given in the global system.

Input File Usage: \*NODE OUTPUT, GLOBAL=YES

Abaqus/CAE Usage: Step module: history output request editor: Domain: Set: toggle on Use global directions for vector-valued output

<!-- source-page: 674 -->

Obtaining nodal history output in the local directions defined by nodal transformations

You can request vector-valued nodal variables in the local directions defined by nodal transformations.

Input File Usage: \*NODE OUTPUT, GLOBAL=NO

Abaqus/CAE Usage: Step module: history output request editor: Domain: Set: toggle off Use global directions for vector-valued output

# Visualizing boundary conditions

Boundary conditions can be visualized in the Visualization module of Abaqus/CAE by selecting View→ODB Display Options. Click the Entity Display tab in the dialog box that appears.

In an Abaqus/Standard analysis boundary condition information is written to the output database only when some nodal output variables are requested as field output.

# Tracer particle output from Abaqus/Explicit

In Abaqus/Explicit tracer particles can be used to obtain output at specific material points that may not correspond to a fixed location in the mesh if adaptive meshing or an Eulerian mesh is used. Tracer particles follow the material motion throughout an analysis regardless of the mesh motion, which makes them ideal for use with adaptive meshing (see “Defining ALE adaptive mesh domains in Abaqus/Explicit,” Section 12.2.2) and during an Eulerian analysis (see “Eulerian analysis,” Section 14.1.1). Both nodal and element output can be obtained at tracer particles.

# Defining tracer particles

You define the initial location of each tracer particle to be coincident with a node, called the “parent node.” These parent nodes are grouped into a tracer set; you must assign a name to the tracer set when you define the tracer particles. In Eulerian analyses parent nodes grouped into the same tracer set as the connected elements must belong to the same Eulerian section. Tracer particle output is not supported when Eulerian mesh motion is used.

Input File Usage: \*TRACER PARTICLE, TRACER SET=tracer\_set\_name list of parent nodes (either node numbers or node set labels)

Abaqus/CAE Usage: Tracer particles are not supported in Abaqus/CAE.

# Particle birth stages

Sets of tracer particles can be released from the current locations of the parent nodes at multiple times during a step. Each release of tracer particles is referred to as a “particle birth.” After particle birth the tracer particles follow the motion of the associated material regardless of the motion of the mesh. You can indicate the number of particle birth stages in a step, n. One particle birth will occur at the beginning of the step, and the rest of the stages will be evenly spaced throughout the step. If you do not specify a number of particle birth stages, a single particle birth will occur at the beginning of the step.

Input File Usage: \*TRACER PARTICLE, TRACER SET=tracer\_set\_name, PARTICLE BIRTH STAGES=n

<!-- source-page: 675 -->

Abaqus/CAE Usage: Tracer particles are not supported in Abaqus/CAE.

# Tracer particles in the output database

Tracer sets will appear as both node and element sets in the output database. If a tracer set has multiple birth stages, additional node and element sets will be created that group all the tracer particles associated with a given birth stage. These subsets are named by appending the birth stage number to the tracer set name. For example, if a tracer set with the name INLET is defined with two particle birth stages, three node sets and three element sets will be created in the output database: INLET Stage 1, INLET Stage 2, and INLET (which contains all the nodes/elements from both INLET Stage 1 and INLET Stage 2).

When tracer particles are used with adaptive meshing, internal field output requests are generated automatically for the requested output variables for all the elements or nodes in the domain that completely defines the space of possible tracer particle locations. This region is determined by Abaqus/Explicit and typically corresponds to the elements attached to the parent nodes and any intersecting adaptive mesh domains. The postprocessing calculator (see “The postprocessing calculator,” Section 4.3.1) will compute the value of any requested output quantity at a tracer particle by interpolating the results from the element that encompasses the particle at the time of output.

When tracer particles are used in an Eulerian analysis, Abaqus/Explicit processes the output requests in the same way as for other node and element output; therefore, the postprocessing calculator is not used, and no additional internal requests are generated.

# Requesting output at tracer particles

You can request element or nodal output for a particular tracer set. Output will be given for all tracer particles that are associated with the specified tracer set name.

Input File Usage: Use one of the following options:

\*NODE OUTPUT, TRACER SET=tracer\_set\_name

\*ELEMENT OUTPUT, TRACER SET=tracer\_set\_name

Abaqus/CAE Usage: Tracer particle output is not supported in Abaqus/CAE.

# Field output at tracer particles

Displacement is the only valid field request for tracer particles. You can obtain the positions of the tracer particles in a specific tracer set by requesting displacements as nodal field output. Tracer particle displacements are output automatically if displacement output is requested for the entire model. You can use the node and element sets created for tracer particles in the output database to control the display of tracer particles in the Visualization module of Abaqus/CAE.

Input File Usage: Use both of the following options:

\*OUTPUT, FIELD

\*NODE OUTPUT, TRACER SET=tracer\_set\_name

U

Abaqus/CAE Usage: Tracer particle output is not supported in Abaqus/CAE.

<!-- source-page: 676 -->

# History output at tracer particles

Requesting history output for tracer particles is similar to requesting history output for elements and nodes. Any valid element integration point variable can be requested. U, V, A, and COORD are the only valid nodal requests. Whole element variables and element section variables cannot be requested. History data are available for a tracer particle only after its birth. When tracer particles are used in an Eulerian analysis, PRESS is the only valid element request.

When tracer particles are used with adaptive meshing, tracer particle history output request triggers an internal field output request for the desired variables for all the elements or nodes in the domain that completely defines the space of possible tracer particle locations.

Input File Usage: Use the following options:

```sql
*OUTPUT, HISTORY
*NODE OUTPUT, TRACER SET=tracer_set_name
*ELEMENT OUTPUT, TRACER SET=tracer_set_name 
```

Abaqus/CAE Usage: Tracer particle output is not supported in Abaqus/CAE.

# Tracer particle propagation in multiple steps

Once defined, all tracer particles remain active in subsequent steps. However, no further particle births occur in the steps that follow the tracer set definition. You can define new tracer particles in subsequent steps by specifying a new tracer set name. The same tracer set name cannot be used more than once within an analysis.

# Tracer particle deactivation

When used with adaptive meshing, individual tracer particles are deactivated if they flow out of the mesh across an Eulerian boundary or are currently tracking material points inside a failed element that has been deleted from the mesh. History data for tracer particles are zero at all times after deactivation.

When used in an Eulerian analysis, individual tracer particles are deactivated when they reach the Eulerian mesh boundary. They are also deactivated if the elements containing these tracer particles become void, which is usually caused by accumulated numerical error during interface reconstruction. Deactivated tracer particles have zero displacement.

# Controlling the output frequency at tracer particles

The frequency of tracer particle output is controlled as described above in “Controlling the output frequency.”

WARNING: When tracer particles are used with adaptive meshing, requesting tracer set history output at a high frequency may cause the output database (.odb) to become large. The disk space required to store the field data is directly proportional to the size of the adaptive mesh domain and the number of tracer sets. The disk space usage is independent of the number of tracer particles in a tracer set. The output database file size is reduced after the postanalysis calculation is performed.

<!-- source-page: 677 -->

In Abaqus/Explicit integrated output can be requested either over a surface or over an element set; in Abaqus/Standard integrated output can be requested over a surface. An integrated output request is used to write the time history of variables such as the total force transmitted across a surface, the total mass of an element set, or the percentage change of the total mass of an element set.

# Selecting the integrated output variables

The integrated variables that can be written to the output database in Abaqus/Explicit are defined in the “Integrated variables” section of “Abaqus/Explicit output variable identifiers,” Section 4.2.2. The integrated variables that can be written to the output database in Abaqus/Standard are defined in the “Section variables” section of “Abaqus/Standard output variable identifiers,” Section 4.2.1.

Input File Usage: \*INTEGRATED OUTPUT list of output variables

Abaqus/CAE Usage: Step module: history output request editor: Select from list below

# Selecting the surface over which integrated output is required

You can specify the surface directly for an integrated output request. Alternatively, you can associate an integrated output section that identifies the surface (see “Integrated output section definition,” Section 2.5.1) with the integrated output request.

Integrated output can be requested for a surface that includes facets, edges, or ends of various types of deformable elements. The surface can include facets of three-dimensional solid elements and continuum shell elements; edges of two-dimensional solid elements, membrane elements, conventional shell, and surface elements; and ends of beam elements, pipe elements, and truss elements.

# Specifying the surface for integrated output directly

If you specify the surface for an integrated output request directly, any vector output variables are given with respect to a fixed global coordinate system and the total moment transmitted across the surface, SOM, is computed about the fixed global origin. See “Element-based surface definition,” Section 2.3.2, for information on defining element-based surfaces.

Input File Usage: Use both of the following options:

\*SURFACE, NAME=surface\_name, TYPE=ELEMENT\*INTEGRATED OUTPUT, SURFACE=surface\_name

Abaqus/CAE Usage: You cannot specify the surface for an integrated output request directly in Abaqus/CAE; you must create an integrated output section as described below.

# Specifying the surface through an integrated output section definition

If you associate an integrated output section definition with an integrated output request, the integrated output variables can be obtained in a local coordinate system that can translate and/or rotate with the deformation (see Figure 4.1.3–1). In addition, the total moment transmitted across the surface, SOM, can be computed about a moving location.

<!-- source-page: 678 -->

![](images/page-678_318e0c3e9683f64fb7a3e564b6d3363cf8ef586a9266e5befa29a18e7a93b5f7.jpg)

<details>
<summary>text_image</summary>

defined section
anchor point
1
2
Y
X
Y
2D
anchor point
1
3
b
2
a
Z
Y
X
defined section
3D
</details>

Figure 4.1.3–1 A user-defined local coordinate system.   
```txt
Input File Usage: Use both of the following options:
*INTEGRATED OUTPUT SECTION, NAME=section_name,
SURFACE=surface_name
*INTEGRATED OUTPUT, SECTION=section_name
Abaqus/CAE Usage: Step module:
Output→Integrated Output Sections→Create: Name: section_name:
select regions for the surface
History output request editor: Domain: Integrated output section: section_name 
```

# Requesting integrated output for “force-flow” studies

To study the “force-flow” through various paths in a model, you must create interior surfaces that cut through one or more regions (similar to a cross-section) so that you can request integrated output of the total force transmitted across these surfaces. You can create such interior surfaces over the element facets, edges, or ends by simply cutting through one or more regions of the model with a plane; see “Creating interior cross-section surfaces” in “Element-based surface definition,” Section 2.3.2, for more information.

<!-- source-page: 679 -->

Input File Usage: Use both of the following options:

\*SURFACE, NAME=surface\_name, TYPE=CUTTING SURFACE

\*INTEGRATED OUTPUT, SURFACE=surface\_name

Abaqus/CAE Usage: You cannot specify the surface for an integrated output request directly in Abaqus/CAE; you must create an integrated output section as described above.

# Requesting integrated output over an element set in Abaqus/Explicit

You can request integrated output over an element set to output its total mass, the percentage change of its total mass, its average rigid body motion or any combination of these variables. The element set must have been defined previously, and it can include any type of elements.

Input File Usage: Use the following option to request integrated output over an element set:

\*INTEGRATED OUTPUT, ELSET=element set name

Abaqus/CAE Usage: Requesting integrated output over an element set is not supported in Abaqus/CAE.

# Controlling the output frequency

The frequency of integrated output is controlled as described above in “Controlling the output frequency.

# Requesting preselected output

Preselected output variables are available only when the integrated output is requested over a surface. If integrated output is requested over an element set, you must specify the variables on the data line.

If the integrated output is requested over a surface, you can request the preselected integrated output variables SOF and SOM. In this case you can also specify additional variables as part of the output request. Alternatively, you can request all integrated variables applicable to the current procedure type. In this case any additional variables that you specify are ignored. If you do not request the preselected variables or all variables, you must specify the variables individually.

Input File Usage: Use the following option to request the preselected integrated output variables:

\*INTEGRATED OUTPUT, VARIABLE=PRESELECT

optional additional variables

Use the following option to request all integrated output variables relevant to the current procedure type:

\*INTEGRATED OUTPUT, VARIABLE=ALL

Use the following option to specify individual integrated output variables:

\*INTEGRATED OUTPUT

individual variables

Abaqus/CAE Usage: Step module: history output request editor: Preselected defaults or All

<!-- source-page: 680 -->

# Limitations when using integrated output requests

Integrated output requests over a surface are subject to the following limitations:

• Integrated output can be requested over a surface that includes facets, edges, or ends of various types of deformable elements. The surface can include facets of three-dimensional solid elements and continuum shell elements; edges of two-dimensional solid elements, membrane elements, conventional shell, and surface elements; and ends of beam elements, pipe elements, and truss elements. The surface should not contain facets of axisymmetric elements or facets of rigid elements.   
• When defining the surface, elements on only one side of the surface must be used. Abaqus/Explicit computes the integrated output variables using the stresses and hourglass-mode forces in elements underlying the surface as in a free-body diagram.   
• The defined surface must cut completely through the mesh, form a closed surface, or be on the exterior of the body. Figure 4.1.3–2 presents some typical cases of valid surfaces. If the surface cuts only partially through the mesh, a valid free-body diagram cannot be isolated (see Figure 4.1.3–3) and incorrect answers may be computed.

![](images/page-680_4586eaafdf7b314a3381098c5bbcdd876e9b011ed1caf8de13aa683b17c097b9.jpg)

<details>
<summary>text_image</summary>

beam
spring A
spring A
pressure load
defined section
elements used to define the section
</details>

Figure 4.1.3–2 Valid section definitions.

• Elements attached to the surface can be on either side of the surface but must not cross the defined surface. Figure 4.1.3–3 presents a few invalid cases.   
• The total force and the total moment in the section are computed based only on the stresses (internal forces) in the identified elements. Thus, inaccurate results may be obtained if distributed body loads are present in these elements since their effect on the total force in the section is not included. Common examples are the inertial loading in dynamic analyses, gravity loads, distributed body forces, and centrifugal loads. In these cases the total force in the section may depend on the choice of elements used to define the section as illustrated in Figure 4.1.3–4(a). Assuming that gravity loading is the only active load, the element stresses will be different in the two elements. Hence,
