Contact surface output, element output, nodal output, and radiation output are available as field output.

*OUTPUT, FIELD
*CONTACT OUTPUT
*ELEMENT OUTPUT
*NODE OUTPUT
*RADIATION OUTPUT

Contact surface output, element output, energy output, integrated output, time incrementation output, fastener interaction output, modal output, nodal output, and radiation output are available as history output.

Requesting large amounts of history output (more than 1000 output requests) may cause performance to degrade in ABAQUS/Standard and will cause performance to degrade in ABAQUS/Explicit. For vector- or tensor-valued output variables each component is considered to be a single request. In the case of element variables history output will be generated at each integration point. For example, requesting history output of the tensor variable S (stress) for a C3D10M element will generate 24 history output requests: (6 components) × (4 integration points). When requesting history output of vector- and tensor-valued variables, it is recommended that individual components be selected where available.

*OUTPUT, HISTORY
*CONTACT OUTPUT
*ELEMENT OUTPUT
*ENERGY OUTPUT
*INTEGRATED OUTPUT
*INCREMENTATION OUTPUT
*INTERACTION OUTPUT
*MODAL OUTPUT
*NODE OUTPUT
*RADIATION OUTPUT

By default, a subset of the diagnostic information that is written to the message file for ABAQUS/Standard analyses is also written to the output database. You can use the Visualization module of ABAQUS/CAE to view this diagnostic information interactively, highlighting problematic areas on a view of the model and using them to resolve errors and warnings in the analysis. For more information, see “The ABAQUS/Standard message file” in “Output,” Section 4.1.1, and Chapter 23, “Viewing diagnostic output,” of the ABAQUS/CAE User's Manual.

*OUTPUT, DIAGNOSTICS=YES

*OUTPUT, DIAGNOSTICS=NO

In ABAQUS/Standard you can specify the output frequency in terms of increments, the number of intervals during the step, the size of regular time intervals throughout the step, or time points throughout the step.

If output is requested at exact time intervals or exact time points, ABAQUS/Standard will obtain a solution corresponding to each output request time. In this case if the frequency of output to the output database file is high, the number of increments and, consequently, the computational cost of the analysis may increase considerably.

History output in ABAQUS/Standard is buffered and is written to disk only after every 10 increments of history data output or when a step has completed. Therefore, history results may not be available immediately for postprocessing.

*OUTPUT, FIELD, FREQUENCY=n 
*OUTPUT, HISTORY, FREQUENCY=n

*OUTPUT, FIELD, NUMBER INTERVAL=n, TIME MARKS=YES
*OUTPUT, HISTORY, NUMBER INTERVAL=n, TIME MARKS=YES

*OUTPUT, FIELD, NUMBER INTERVAL=n, TIME MARKS=NO
*OUTPUT, HISTORY, NUMBER INTERVAL=n, TIME MARKS=NO

*OUTPUT, FIELD, TIME INTERVAL=t , TIME MARKS=YES
*OUTPUT, HISTORY, TIME INTERVAL=t, TIME MARKS=YES

*OUTPUT, FIELD, TIME INTERVAL=t , TIME MARKS=NO
*OUTPUT, HISTORY, TIME INTERVAL=t, TIME MARKS=NO

Specifying output frequency in time points

You can write the results at specified time points throughout the step.

By default, ABAQUS/Standard adjusts the time increment (in some cases ABAQUS/Standard might violate the minimum time increment specified) to ensure that data are written at the exact time points specified. Alternatively, you can specify that the data be written immediately after each time point. In this case no adjustment of the time increment is necessary.

You can specify the output frequency in time points only for the combinations of procedures and time incrementation methods specified in Table 4.1.3–1. In addition, this capability is not supported for linear perturbation analyses, except for modal dynamic analysis (“Transient modal dynamic analysis,” Section 6.3.7).

Input File Usage:

Use the first option with one of the subsequent options to request results at the exact time points:

*TIME POINTS, NAME=time points name *OUTPUT, FIELD, TIME POINTS=time points name, TIME MARKS=YES *OUTPUT, HISTORY, TIME POINTS=time points name, TIME MARKS=YES Use the first option with one of the subsequent options to request results at the increments ending immediately after each time point: *TIME POINTS, NAME=time points name *OUTPUT, FIELD, TIME POINTS=time points name, TIME MARKS=NO *OUTPUT, HISTORY, TIME POINTS=time points name, TIME MARKS=NO

ABAQUS/CAE Usage:	Use the following option to request results at the exact time points:
	Step module: field or history output request editor: Including specific time points, At Exact times indicated by the intervals Use the following option to request results at the increments ending immediately after each time point: Step module: field or history output request editor: Including specific time points, At Approximate times indicated by the intervals

Table 4.1.3–1 ABAQUS/Standard procedures that support output frequency control using number of intervals, time intervals, or time points.

Procedure	Time incrementation	Output frequency
		at exact times	immediately after each time mark
“Static stress analysis,” Section 6.2.2 (except if the Riks method is used)	Automatic
	Fixed	—
“Implicit dynamic analysis using direct integration,” Section 6.3.2	Automatic
	Fixed	—
“Uncoupled heat transfer analysis,” Section 6.5.2 (output frequency in number intervals is not supported if you specify that the analysis end when steady state is reached)	Automatic
	Fixed	—
“Mass diffusion analysis,” Section 6.8.1 (output frequency in number intervals is not supported if you specify that the analysis end when steady state is reached)	Automatic
	Fixed	—
“Coupled pore fluid diffusion and stress analysis,” Section 6.7.1 (output frequency in number intervals is not supported if you specify that the analysis end when steady state is reached)	Automatic
	Fixed	—
“Fully coupled thermal-stress analysis,” Section 6.5.4	Automatic
	Fixed	—
“Coupled thermal-electrical analysis,” Section 6.6.2 (output frequency in number intervals is not supported if you specify that the analysis end when steady state is reached)	Automatic
	Fixed	—
“Steady-state transport analysis,” Section 6.4.1	Automatic
	Fixed	—
“Subspace-based steady-state dynamic analysis,” Section 6.3.9	Fixed	—
“Quasi-static analysis,” Section 6.2.5	Automatic
	Fixed	—
“Transient modal dynamic analysis,” Section 6.3.7	Fixed	—

Field output data are always written at the start and end of each step in which the output request is active. In addition, you can specify the output frequency in terms of the number of intervals during the step, the size of regular time intervals throughout the step, or time points throughout the step. The times at which the results are written are referred to as time marks.

*OUTPUT, FIELD, NUMBER INTERVAL=n, TIME MARKS=NO

*OUTPUT, FIELD, NUMBER INTERVAL=n, TIME MARKS=YES

*OUTPUT, FIELD, TIME INTERVAL=t

*TIME POINTS, NAME=time points name 
*OUTPUT, FIELD, TIME POINTS=time points name, TIME MARKS=YES

*TIME POINTS, NAME=time points name 
*OUTPUT, FIELD, TIME POINTS=time points name, TIME MARKS=NO

If history output is selected, you can specify the output frequency in terms of either increments or regular intervals throughout the step.

*OUTPUT, HISTORY, FREQUENCY=n

*OUTPUT, HISTORY, TIME INTERVAL=t

By default, all output requests defined in previous steps are removed when new requests are defined, regardless of the type of output request being defined. In other words, a new field output request in a step removes all field and history output requests defined in previous steps. Only output requests defined in previous steps are affected; other output requests defined in the same step are not affected.

This behavior is the same as the behavior for output requests to the ABAQUS/Standard data file (file_name.dat) and the ABAQUS/Standard and ABAQUS/Explicit results files (file_name.fil); see “Output to the data and results files,” Section 4.1.2.

Because all existing output requests are removed when a new request is defined in a step, all output requests within the same step are treated as new (i.e., additional output requests or replacement output requests are treated as equivalent to new output requests).

Alternatively, you can specify a new output request without removing all previously defined output requests.

*OUTPUT, FIELD, OP=NEW
*OUTPUT, HISTORY, OP=NEW

*OUTPUT, FIELD, OP=ADD
*OUTPUT, HISTORY, OP=ADD

You can replace an output request of the same type (e.g., field or history) and frequency with a new request. No other previously defined requests will be affected.

You cannot replace an output request to change its frequency. If no matching request is found, the request specified is simply added to the step.

To remove a previously defined request, you can replace the output request without specifying any new output requests.

*OUTPUT, FIELD, OP=REPLACE
*OUTPUT, HISTORY, OP=REPLACE

To suppress completely all output requests that have been defined in previous steps, you can specify an output frequency of 0.

You can activate a procedure-specific set of commonly requested output variables. See Table 4.1.3–2 for a list of procedure types and their accompanying preselected variables. The variables written to the output database may change if the procedure type changes between steps.

If you request preselected field or history output and request additional output variables using individual output requests for specific variable types, the variables requested will be appended to the variables contained in the preselected list.

For geometrically nonlinear analysis in ABAQUS/Standard, E is not available for output and LE is output by default. For linear perturbation analyses and geometrically linear analyses in ABAQUS/Standard, LE and NE strain output requests yield the same output as E. For geometrically linear analysis in ABAQUS/Explicit, LE is output.

ABAQUS may omit some preselected variables from the analysis results. ABAQUS omits preselected output variables if they are not applicable for the element type used to mesh the model or if other factors make the variables unsuitable for the analysis.

*OUTPUT, FIELD, VARIABLE=PRESELECT
*OUTPUT, HISTORY, VARIABLE=PRESELECT

You can request all variables applicable to the current procedure and material type. Any individual output requests for specific variable types are ignored in this case.

*OUTPUT, FIELD, VARIABLE=ALL
*OUTPUT, HISTORY, VARIABLE=ALL

When an ABAQUS/Explicit analysis encounters a fatal error in an increment, the preselected variables applicable to the current procedure are written automatically to the output database as field data. The analysis will go through an additional increment with a zero time increment size before writing these data.

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

*ELEMENT OUTPUT
list of output variables

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.

*ELEMENT OUTPUT, ELSET=element_set_name

*ELEMENT OUTPUT
list of output points
list of output variables

*OUTPUT, FIELD
*ELEMENT OUTPUT, REBAR=rebar_name, ELSET=element_set_name
*OUTPUT, HISTORY
*ELEMENT OUTPUT, REBAR=rebar_name, ELSET=element_set_name

Integration point variables and section variables 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. ABAQUS writes only integration point data to the output database. Transferring of results from the integration points to the user-specified position is done by the postprocessing calculator. See “The postprocessing calculator,” Section 4.3.1, for details. Element history output to the output database is always provided at the integration points.

*ELEMENT OUTPUT, POSITION=INTEGRATION POINTS

*ELEMENT OUTPUT, POSITION=CENTROIDAL

*ELEMENT OUTPUT, POSITION=NODES

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

You can request the preselected, procedure-specific element output variables described in Table 4.1.3–2. 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.

*ELEMENT OUTPUT, VARIABLE=PRESELECT

*ELEMENT OUTPUT, VARIABLE=ALL

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 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 PlotMaterial Orientations in the Visualization module. You can choose to suppress the direction output to the output database.

*ELEMENT OUTPUT, FIELD, DIRECTIONS=NO

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, and “ABAQUS/Explicit output variable identifiers,” Section 4.2.2.

*NODE OUTPUT
list of output variables

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.

*NODE OUTPUT, NSET=node_set_name

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

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

You can request the preselected, procedure-specific nodal output variables described in Table 4.1.3–2. 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.

*NODE OUTPUT, VARIABLE=PRESELECT

*NODE OUTPUT, VARIABLE=ALL

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 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.

Boundary conditions can be visualized in the Visualization module of ABAQUS/CAE by selecting ViewODB 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.

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.

*TRACER PARTICLE, TRACER SET=tracer_set_name
list of parent nodes (either node numbers or node set labels)

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.

*TRACER PARTICLE, TRACER SET=tracer_set_name, PARTICLE BIRTH STAGES=n

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).

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.

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.

*NODE OUTPUT, TRACER SET=tracer_set_name 
*ELEMENT OUTPUT, TRACER SET=tracer_set_name

*OUTPUT, FIELD
*NODE OUTPUT, TRACER SET=tracer_set_name 
U

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

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.

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.

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

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

*INTEGRATED OUTPUT
list of output variables

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 and truss elements.

*SURFACE, NAME=surface_name, TYPE=ELEMENT
*INTEGRATED OUTPUT, SURFACE=surface_name

*INTEGRATED OUTPUT SECTION, NAME=section_name, SURFACE=surface_name
*INTEGRATED OUTPUT, SECTION=section_name

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 “Defining element-based surfaces,” Section 2.3.2, for more information.

*SURFACE, NAME=surface_name, TYPE=CUTTING SURFACE
*INTEGRATED OUTPUT, SURFACE=surface_name

The frequency of integrated output is controlled as described above in “Controlling the output frequency for history output in ABAQUS/Explicit.”

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.

*INTEGRATED OUTPUT, VARIABLE=PRESELECT 
optional additional variables

*INTEGRATED OUTPUT, VARIABLE=ALL

*INTEGRATED OUTPUT
individual variables

Integrated output requests are subject to the following limitations:

The energy variables that can be written to the output database are defined in the “Total energy output quantities” section of “ABAQUS/Standard output variable identifiers,” Section 4.2.1, and “ABAQUS/Explicit output variable identifiers,” Section 4.2.2.

*ENERGY OUTPUT
list of output variables

You can specify the element set for which total energy output is being requested. In this case the energies are summed for all the elements in the specified set. You cannot specify an element set for the following procedures:

The following energies are not available as element set quantities: ALLWK, ALLFD, ALLQB, ALLKL, ALLFC, and ETOTAL.

If you do not specify an element set, the total energies for the whole model will be output. If total energy output for both the whole model and for different element sets is desired, the energy output requests must be repeated: once without a specified element set to request energy output for the whole model and once for each specified element set.

*ENERGY OUTPUT, ELSET=element_set_name

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

You can request the preselected, procedure-specific energy output variables described in Table 4.1.3–2. In this case you can specify additional variables as part of the output request.

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

*ENERGY OUTPUT, VARIABLE=PRESELECT

*ENERGY OUTPUT, VARIABLE=ALL

You can define three types of low-pass Infinite Impulse Response filters as part of the model definition. Typical magnitude curves for analog type filters are presented in Figure 4.1.3–5.

To define a Butterworth filter, you must specify the cutoff frequency, , and the filter order, N. Since the implementation of the filters is done using cascades of second-order sections, ABAQUS expects an even number for the filter order. If you specify an odd number for the order, the order will be changed internally to the closest greater even number. The default value for the order is two, and the highest order that can be prescribed is twenty. For the Chebyshev filters you must also specify an additional parameter, the ripple factor. The ripple factor is equal to for a Type I Chebyshev filter and is equal to for a Type II Chebyshev filter (see Figure 4.1.3–5).

No checks are performed to ensure that the cutoff frequency is appropriate; for example, ABAQUS does not check that only the noise of the signal is eliminated. You need to know the range of the physical frequencies that are expected in the solution, and you must prescribe a cutoff frequency greater than these frequencies. In addition, the cutoff frequency should be less than half the sampling frequency (the sampling frequency is the inverse of the time increment); otherwise, no filtering is performed. The values of variables at time zero (zero increment) are used as the initial conditions (or start-up conditions). The filtered history output variables are continuous over the steps; i.e., the start-up conditions are used only in the first step.

You must assign each filter definition a name that can be used to refer to the filter from an output request.

*FILTER, NAME=filter_name, TYPE=BUTTERWORTH 
*FILTER, NAME=filter_name, TYPE=CHEBYS1
*FILTER, NAME=filter_name, TYPE=CHEBYS2

To pre-filter element, nodal, contact, integrated, or fastener interaction history output based on one of the low-pass Infinite Impulse Response filters that you defined, you refer to this filter by name from the output request.

*OUTPUT, HISTORY, FILTER=filter_name

You can request that ABAQUS/Explicit create an anti-aliasing filter internally based on the sampling interval that is specified in the history output request. In this case a filter definition is not required. The anti-aliasing filter is a second order Butterworth type, for which the cutoff frequency is set internally to one-third of the sampling frequency. In this case the sampling frequency is the inverse of the time interval, t, used for the history output.

*OUTPUT, HISTORY, FILTER=ANTIALIASING, TIME INTERVAL=t

The modal variables that can be written to the output database are defined in the “Modal variables” section of “ABAQUS/Standard output variable identifiers,” Section 4.2.1.

*MODAL OUTPUT
list of output variables

The frequency of modal output is controlled as described above in “Controlling the output frequency in ABAQUS/Standard.”

You can choose to request all modal variables applicable to the current procedure and material type. In this case any additional variables you specify are ignored.

*MODAL OUTPUT, VARIABLE=ALL

The surface variables that can be written to the output database are listed in the “Surface variables” section of “ABAQUS/Standard output variable identifiers,” Section 4.2.1, and “ABAQUS/Explicit output variable identifiers,” Section 4.2.2.

*CONTACT OUTPUT
list of output variables

In ABAQUS/Standard you can select the master and slave surfaces for which output is required, and you can specify a subset of slave nodes for output in addition to the master and slave surfaces or independently. If no surfaces or slave nodes are specified, surface variables are written for all the contact pairs in the model. If you specify the slave surface but not the master surface, output is written for all contact pairs that involve the specified slave surface.

*CONTACT OUTPUT, MASTER=master, SLAVE=slave, NSET=node_set_name

In ABAQUS/Explicit you can select the contact pairs for which surface output is desired. Surface output is contact pair-specific, so that contact output for a particular surface involved in a selected contact pair will include only the contributions from that contact pair if the surface is involved in multiple contact pairs. Surface output is available only for discrete (node-based or element-based) surfaces; it is not available for any analytical surfaces within a contact pair.

Alternatively, you can select the fastened node sets for which output is desired. You cannot select both contact pairs and fastened node sets in the same surface output request.

If no contact pairs or fastened node sets are specified and you do not activate the surface output request for the entire general contact domain (as described below), surface variables are written for all the contact pairs in the model and the general contact domain (if it is defined).

*CONTACT OUTPUT, CPSET=contact_pair_set_name

*CONTACT OUTPUT, NSET=node_set_name

If the surfaces of a contact pair overlap with the general contact domain, general contact results will still be output for the contact pair surfaces. However, those results exclude contributions from the contact pair interactions.

*CONTACT OUTPUT, GENERAL CONTACT

*CONTACT OUTPUT, SURFACE=surface_name

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

You can request the preselected, procedure-specific surface output variables described in Table 4.1.3–2. In this case you can specify additional variables as part of the output request.

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

*CONTACT OUTPUT, VARIABLE=PRESELECT

*CONTACT OUTPUT, VARIABLE=ALL

The available incrementation output variables are the ABAQUS/Explicit time increment size, DT; the percent change in mass of the model due to mass scaling, DMASS; and the steady-state detection variables SSPEEQ, SSSPRD, SSFORC, and SSTORQ.

*INCREMENTATION OUTPUT
list of output variables

The frequency of incrementation output is controlled as described above in “Controlling the output frequency for history output in ABAQUS/Explicit.”

You can request the preselected, procedure-specific incrementation output variables. In this case you can specify additional variables as part of the output request.

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

*INCREMENTATION OUTPUT, VARIABLE=PRESELECT

*INCREMENTATION OUTPUT, VARIABLE=ALL

The fastener interaction variables that can be written to the output database are listed in the “Fastener interaction variables” section of “ABAQUS/Standard output variable identifiers,” Section 4.2.1, and “ABAQUS/Explicit output variable identifiers,” Section 4.2.2.

*INTERACTION OUTPUT
list of output variables

You can request output for all fasteners associated with a given fastener interaction or all fasteners associated with a given set of fastener reference nodes.

If you specify a fastener interaction name, the requested output will be written for all fastener layers associated with the specified fastener interaction.

If you specify a node set, any nodes in the node set that are not fastener reference nodes will be ignored.

*INTERACTION OUTPUT, NAME=fastener_interaction_name

*INTERACTION OUTPUT,  NSET=node_set_name

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

There are no preselected variables for fastener interaction output.

The radiation output variables that can be written to the output database are listed in the “Cavity radiation variables” section of “ABAQUS/Standard output variable identifiers,” Section 4.2.1.

*RADIATION OUTPUT
list of output variables

You can specify the cavity, element set, or surface for which radiation output is required. Each radiation output request can apply to only one type of region. If you do not specify a region of the model, radiation variables are output for all the cavities in the model.

*RADIATION OUTPUT, CAVITY=cavity_name
*RADIATION OUTPUT, ELSET=element_set_name
*RADIATION OUTPUT, SURFACE=surface_name

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

You can request all radiation variables applicable to the current procedure. In this case any additional variables you specify are ignored.

*RADIATION OUTPUT, VARIABLE=ALL

The input listing below will produce both field and history output for Step 1. Field output will be written every 2 increments. This field output request consists of preselected element variables for the whole model, as well as the variable PEQC. In addition, plastic strains will be written out for element set SMALL, and the nodal variables U and RF will be written to the output database for node set NSMALL. History output will be written every increment. The variables ALLKE, ALLSE, and ALLWK will be written for the whole model. In addition, ALLPD will be written for element set SMALL.

In Step 2 the history output request defined in Step 1 is replaced by a request for the energy variables ALLKE, ALLPD, and ALLSE for element set SMALL. The history output request defined in Step 1 is removed. The field output request defined in Step 1 is passed into Step 2 unchanged, but another field output request for element energies at every increment is added.

*STEP
*STATIC
...
...
*OUTPUT, FIELD, FREQUENCY=2
*ELEMENT OUTPUT, VARIABLE=PRESELECT
PEQC,
*ELEMENT OUTPUT, ELSET=SMALL
PE,
*NODE OUTPUT, NSET=NSMALL
U, RF
*OUTPUT, HISTORY, FREQUENCY=1
*ENERGY OUTPUT
ALLKE, ALLSE, ALLWK
*ENERGY OUTPUT, ELSET=SMALL
ALLPD
*END STEP
*STEP
*STATIC
...
...
*OUTPUT, HISTORY, OP=REPLACE, FREQUENCY=1
*ENERGY OUTPUT, ELSET=SMALL
ALLKE, ALLPD, ALLSE
*OUTPUT, FIELD, OP=ADD, FREQUENCY=1
*ELEMENT OUTPUT
ELEN
*END STEP

The input listing below will produce both field and history output for Step 1. Field output will be written at 5 equally spaced intervals, and the time marks will be hit exactly. This field output request consists of preselected element variables for the whole model, as well as the variable PEQC. In addition, plastic strains will be written out for element set SMALL, and the nodal variables U and RF will be written to the output database for node set NSMALL. History output will be written at a time interval of 0.005. The ABAQUS/Explicit time step, DT, will be written, along with the variables ALLKE, ALLSE, and ALLWK for the whole model. The output variables SOAREA and SOF integrated over the surface CROSS_SECTION1 will be written. The preselected variables SOF and SOM integrated over the surface CROSS_SECTION2 defined by the integrated output section SECTION1 will be written in the local coordinate system LOCALSYSTEM. In addition, ALLPD will be written for element set SMALL.

In Step 2 the history output request defined in Step 1 is replaced by a request for the energy variables ALLKE, ALLPD, and ALLSE for element set SMALL. The history output request defined in Step 1 is removed. The field output request defined in Step 1 is passed into Step 2 unchanged, but another field output request for element energies at 10 equally spaced intervals is added.

*STEP
*DYNAMIC, EXPLICIT,.1...
...
*OUTPUT, FIELD, NUMBER INTERVAL=5, TIME MARKS=YES
*ELEMENT OUTPUT, VARIABLE=PRESELECT
PEQC,
*ELEMENT OUTPUT, ELSET=SMALL
PE,
*NODE OUTPUT, NSET=NSMALL
U, RF
*OUTPUT, HISTORY, TIME INTERVAL=0.005
*INCREMENTATION OUTPUT
DT
*ENERGY OUTPUT
ALLKE, ALLSE, ALLWK
*ENERGY OUTPUT, ELSET=SMALL
ALLPD
*INTEGRATED OUTPUT, SURFACE=CROSS_SECTION1
SOF, SOAREA
*INTEGRATED OUTPUT SECTION, NAME=SECTION1, 
SURFACE=CROSS_SECTION2, ORIENTATION=LOCALSYSTEM 
*INTEGRATED OUTPUT, SECTION=SECTION1, VARIABLE=PRESELECT 
*END STEP
*STEP
*DYNAMIC, EXPLICIT,.1...
...
*OUTPUT, HISTORY, OP=REPLACE, TIME INTERVAL=0.005
*ENERGY OUTPUT, ELSET=SMALL
ALLKE, ALLPD, ALLSE
*OUTPUT, FIELD, OP=ADD, NUMBER INTERVAL=10
*ELEMENT OUTPUT
ELEN
*END STEP