Output to the Output Database

Contact surface output, element output, nodal output, and radiation output are available as field output in Abaqus/Standard and Abaqus/Explicit.

OUTPUT, FIELD
CONTACT OUTPUT
ELEMENT OUTPUT
NODE OUTPUT
RADIATION OUTPUT

Step module: field output request editor

Contact surface output, element output, energy output, integrated output, time incrementation output, modal output, nodal output, and radiation output are available as history output in Abaqus/Standard and Abaqus/Explicit.

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
MODAL OUTPUT
NODE OUTPUT
RADIATION OUTPUT

Step module: history output request editor

By default, a subset of the diagnostic information that is written to the message file for Abaqus/Standard analyses and to the status and message files for Abaqus/Explicit 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 message file in Abaqus/Standard and Abaqus/Explicit, and Viewing diagnostic output.

OUTPUT, DIAGNOSTICS=YES

OUTPUT, DIAGNOSTICS=NO

Visualization module: ToolsJob Diagnostics

Abaqus/Standard provides several options for controlling the output frequency, depending on whether the analysis is in the time domain (e.g., general statics), frequency domain (e.g., steady state dynamics), or mode domain (e.g., natural frequency extraction). These options can be used to reduce the amount of output written and hence improve performance and disk space use as compared to the default output.

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,  FREQUENCY=n 

Step module: field or history output request editor: Frequency: Every n increments: n

OUTPUT, FIELD, MODE LIST

Step module: field output request editor: Frequency: Specify modes: list of modes

OUTPUT,  FREQUENCY=n

Step module: field or history output request editor: Frequency: Every n increments: n

OUTPUT,  NUMBER INTERVAL=n, TIME MARKS=YES

OUTPUT,  NUMBER INTERVAL=n, TIME MARKS=NO

Step module: field or history output request editor: Frequency: Evenly spaced time intervals, Interval: n, Timing: Output at exact times

Step module: field or history output request editor: Frequency: Evenly spaced time intervals, Interval: n, Timing: Output at approximate times

OUTPUT,  TIME INTERVAL=t , TIME MARKS=YES

OUTPUT,  TIME INTERVAL=t , TIME MARKS=NO

Step module: field or history output request editor: Frequency: Every x units of time: t, Timing: Output at exact times

Step module: field or history output request editor: Frequency: Every x units of time: t, Timing: Output at approximate times

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

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

Step module: field or history output request editor: From time points, Name: time points name, Timing: Output at exact times

Step module: field or history output request editor: From time points, Name: time points name, Timing: Output at approximate times

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

Step module: field output request editor: Frequency: Evenly spaced time intervals, Interval: n, Timing: Output at approximate times

Step module: field output request editor: Frequency: Evenly spaced time intervals, Interval: n, Timing: Output at exact times

OUTPUT, FIELD, TIME INTERVAL=t

Step module: field output request editor: Frequency: Every x units of time: 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

Step module: field output request editor: Frequency: From time points, Name: time points name, Timing: Output at exact times

Step module: field output request editor: Frequency: From time points, Name: time points name, Timing: Output at approximate times

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

Step module: history output request editor: Frequency: Every n time increments: n

OUTPUT, HISTORY, TIME INTERVAL=t

Step module: history output request editor: Frequency: Every x units of time: 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.

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).

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

Step module: Create Field Output Request or Create History Output Request

Alternatively, you can specify additional output requests without removing all default and previously defined output requests.

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

Step module: Create Field Output Request or Create History Output Request

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 variables.

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

Step module: Field Output Requests Manager or History Output Requests Manager: Edit or Delete

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 1 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

Step module: field or history output request editor: Preselected defaults

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

Step module: field or history output request editor: 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 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.

The element variables that can be written to the output database are defined in Abaqus/Standard output variable identifiers and Abaqus/Explicit output variable identifiers.

ELEMENT OUTPUT
list of output variables

Step module: field or history output request editor: Select from list below 

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

Step module: field or history output request editor: Domain: Set: set_name

ELEMENT OUTPUT, EXTERIOR

Step module: field output request editor: Domain: Whole model; toggle on Exterior only 

ELEMENT OUTPUT
list of output points
list of output variables

Step module: field or history output request editor: Output at shell, beam, and layered section points: Specify: list of output points

ELEMENT OUTPUT, ALLSECTIONPTS

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

Step module: field or history output request editor: Output for rebar: Include

Step module: field or history output request editor: Output for rebar: Only

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.

ELEMENT OUTPUT, POSITION=INTEGRATION POINTS

ELEMENT OUTPUT, POSITION=CENTROIDAL

ELEMENT OUTPUT, POSITION=NODES

ELEMENT OUTPUT, POSITION=AVERAGED AT NODES

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

The precision of element output is controlled as described above in Controlling the precision.

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

ELEMENT OUTPUT, VARIABLE=PRESELECT

ELEMENT OUTPUT, VARIABLE=ALL

Step module: field or history output request editor: Preselected defaults or 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: 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 PlotMaterial Orientations in the Visualization module. You can choose to suppress the direction output to the output database.

ELEMENT OUTPUT, DIRECTIONS=NO

Step module: field output request editor: toggle off Include local coordinate directions when available

The nodal variables that can be written to the output database are defined in the Nodal variables section of Abaqus/Standard output variable identifiers and Abaqus/Explicit output variable identifiers.

NODE OUTPUT
list of output variables

Step module: field or history output request editor: Select from list below 

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

Step module: field or history output request editor: Domain: Set: set_name

NODE OUTPUT, EXTERIOR

Step module: field output request editor: Domain: Whole model; toggle on Exterior only 

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

The precision of nodal output is controlled as described above in Controlling the precision.

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

NODE OUTPUT, VARIABLE=PRESELECT

NODE OUTPUT, VARIABLE=ALL

Step module: field or history output request editor: Preselected defaults or 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 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), 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.

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). In this case you can specify whether output is desired in global or local directions.

NODE OUTPUT, GLOBAL=YES

NODE OUTPUT, GLOBAL=NO

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. 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.

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).

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) 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.

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.

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.

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 in Abaqus/Explicit are defined in the Integrated variables section of Abaqus/Explicit output variable identifiers. 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.

INTEGRATED OUTPUT
list of output variables

Step module: history output request editor: Select from list below 

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) 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.

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

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 1). In addition, the total moment transmitted across the surface, SOM, can be computed about a moving location.

Figure 1. A user-defined local coordinate system.

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:

OutputIntegrated Output SectionsCreate: Name: section_name:
select regions for the surface

History output request editor: Domain: 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 for more information.

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

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.

INTEGRATED OUTPUT, ELSET=element set name

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

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.

INTEGRATED OUTPUT, VARIABLE=PRESELECT 
optional additional variables

INTEGRATED OUTPUT, VARIABLE=ALL

INTEGRATED OUTPUT
individual variables

Step module: history output request editor: Preselected defaults or All

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 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 3) and incorrect answers may be computed.

  Figure 2. Valid section definitions.
  
  
  Figure 3. Invalid section definitions.
  
  

• Elements attached to the surface can be on either side of the surface but must not cross the defined surface. Figure 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(a).

  Figure 4. Total force in the section.
  
  

  Assuming that gravity loading is the only active load, the element stresses will be different in the two elements. Hence, if the same surface is defined first using element 1 and then using element 2, different answers for the total force will be obtained. In a similar way the effects of any distributed body fluxes (heat, electrical, etc.) prescribed in the identified elements are not included.

• Depending on which side of the surface is used to define the section, different answers will be obtained in analyses similar to the case illustrated in Figure 4(b). Assuming a quasi-static analysis with the concentrated loads shown in the figure being the only active loads, a zero total force is reported if the surface is defined using element 1 and a nonzero force equal to the sum of the concentrated loads is obtained if the surface is defined using element 2.

The energy variables that can be written to the output database are defined for Abaqus/Standard in Total energy output quantities and for Abaqus/Explicit in Total energy output.

ENERGY OUTPUT
list of output variables

Step module: history output request editor: Select from list below 

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:

• Transient modal dynamic analysis

• Response spectrum analysis

• Random response analysis

The following energies are not available as element set quantities: ALLCCDW, ALLCCE, ALLCCEN, ALLCCET, ALLCCSD, ALLCCSDN, ALLCCSDT, ALLFC, ALLFD, ALLKL, ALLQB, ALLWK, ALLVDM, ALLHDM, 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

Step module: history output request editor: Domain: Set: 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 1. 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

Step module: history output request editor: Preselected defaults or 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 5, where ${\mathrm{\Omega }}_c$ represents the normalized cutoff frequency, which is the ratio of the cutoff frequency to the sampling frequency (the sampling frequency is the inverse of the time increment).

Figure 5. Typical magnitude curves for low-pass filters.

The Butterworth filter is very common; its response in the pass band is known as maximally flat. The Type I Chebyshev filter has a sharper transition between the pass band and the stop band, but it has a ripple in the pass band. The Type II Chebyshev filter also has a sharper transition between the pass band and the stop band than a Butterworth filter of the same order, but it has a ripple in the stop band. The higher the order of the filter, the narrower the transition band. However, the computational cost increases as the order increases. In addition, for high-order filters the phase lag, which is the time delay between the filtered and unfiltered signal, may become significant. For most applications filter orders of two or four are sufficiently accurate.

To define a Butterworth filter, you must specify the cutoff frequency, $f_c$ , 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 increased internally to the next 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 $ϵ$ for a Type I Chebyshev filter and is equal to $1/A$ for a Type II Chebyshev filter (see Figure 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; otherwise, no filtering is performed. Abaqus internally remaps (using a quadratic interpolation) the output raw data so that the filtering can satisfy the constant time-increment (sampling) requirement.

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

Step module: ToolsFilterCreate: Name: filter_name; Butterworth, Type I Chebyshev, or Type II Chebyshev

FILTER, NAME=filter_name, TYPE=filter_type, START CONDITION=DC 

FILTER, NAME=filter_name, TYPE=filter_type, 
START CONDITION=USER DEFINED

To pre-filter element, nodal, contact, or integrated history output or element and nodal field 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, FILTER=filter_name

Step module: field or history output request editor: Apply filter: filter_name

For history output you can request that Abaqus/Explicit create an antialiasing filter that is internally based on the time interval specified in the output request. The cutoff frequency is set internally to one-sixth of the time frequency (the time frequency is the inverse of the time interval, t, used for history output). If no time intervals are specified, the default number of history output intervals is used to create the cutoff frequency of the filter. You can also use antialiasing filters for a field output request, but in this case the cutoff frequency is set to one-sixth of a time frequency corresponding to two hundred time intervals per step if less than two hundred field frames are requested. If more than two hundred field frames are requested, the cutoff frequency is set to one-sixth of the requested time frequency. The antialiasing filter is a second-order Butterworth type and a filter definition is not required.

Abaqus/Explicit does not check whether the specified time interval for history output provides an appropriate cutoff frequency to build the internal filter. You should know approximately how many data points are required to describe your history curve (or signal) accurately, and Abaqus/Explicit will give you the most physical (un-aliased) representation of the signal for that number of points. Similarly for field output Abaqus/Explicit does not check whether the cutoff corresponding to two hundred sampling intervals or more (if you request more than two hundred frames) is appropriate for your analysis. If a lower (or higher) cutoff frequency is needed, you should define the filter in the model data.

OUTPUT, FIELD, FILTER=ANTIALIASING, TIME INTERVAL=t

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

Step module: field or history output request editor: Frequency: Every x units of time: t, Apply filter: Antialiasing

OUTPUT, FIELD, FILTER=ANTIALIASING, NUMBER INTERVAL=n

Step module: field output request editor: Frequency: Evenly spaced time intervals, Interval: n, Apply filter: Antialiasing

You can apply a filter to a field output request or a history output request to obtain the maximum, minimum, or absolute maximum values for each variable in the output request. The absolute maximum option enables you to obtain the largest absolute value, negative or positive, for each variable in the output request. Abaqus evaluates maximum, minimum, or absolute maximum values at every increment during the analysis and reports these values at the time given by the output interval specified in the output request. For field output requests the last output frame will contain the maximum (or absolute maximum) value and minimum value over the entire step; the intermediate frames will show the maximum, minimum, or absolute maximum value up to the frame time. An additional output variable containing the time when the maximum, minimum, or absolute maximum occurred is output automatically for each output variable requested. This time output is written by default (and it cannot be suppressed).

For field output requests Abaqus filters by default each component of tensor and vector quantities of output variable independently and provides separate maximum, minimum, or absolute maximum values for each component of the variable. You can, however, request the maximum or minimum value or apply a limit value to an invariant such as Mises stress for element output or magnitude for nodal output (see Applying bounding values to invariants below).

FILTER, TYPE=filter_type, OPERATOR=MAX
FILTER, TYPE=filter_type, OPERATOR=MIN
FILTER, TYPE=filter_type, OPERATOR=ABSMAX

FILTER, OPERATOR=MAX
FILTER, OPERATOR=MIN
FILTER, OPERATOR=ABSMAX

You can apply a filter to a field output request or a history output request to prescribe a bounding value for the variables in the output request. If any of the variables in the output request reach a value higher than the maximum limit, lower than the minimum limit, or greater than the absolute maximum limit, Abaqus returns the limiting value. The time at which the limit was reached is output separately for each requested variable. This time output is written by default (and it cannot be suppressed).

FILTER, TYPE=filter_type, OPERATOR=operator_type, LIMIT=value

FILTER, OPERATOR=operator_type, LIMIT=value

You can apply a filter to a field output request or a history output request that stops the analysis when the value of any variable in the output request reaches a specified upper bound or lower bound.

FILTER, TYPE=filter_type, OPERATOR=operator_type, LIMIT=value, HALT

FILTER, OPERATOR=operator_type, LIMIT=value, HALT

By default, each component of a tensor or vector quantity is filtered individually and the maximum, minimum, or absolute maximum value and the limiting values are reported separately for each component. You can, however, apply a filter directly to an invariant. In this case Abaqus internally monitors the invariant you specified. Abaqus still writes the components to the output database, but these components correspond to the maximum, minimum, or limiting values of the invariant. Table 2 shows which invariants are available for output variable categories.

FILTER, TYPE=filter_type, OPERATOR=operator_type, LIMIT=value, INVARIANT=FIRST, SECOND, MAXP, INTERMP, or MINP

FILTER, OPERATOR=operator_type, LIMIT=value, INVARIANT= FIRST or SECOND

Low-pass Infinite Impulse Response filters such as Butterworth and Chebyshev filters are intended for filtering of output variables susceptible to noise, such as accelerations and reaction forces or, to a lesser degree, stress and strain. However, digital filtering is allowed for most element and nodal output variables, and you can apply bounding values on unfiltered data for nearly all element and nodal output variables. Table 3 shows the set of output variables that cannot be digitally filtered but to which you can apply bounding values, and Table 4 shows the set of output variables for which neither digital filtering nor application of bounding values are allowed.

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

Step module: history output request editor: 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 and Abaqus/Explicit output variable identifiers.

CONTACT OUTPUT
list of output variables

Step module: field or history output request editor: Select from list below 

Output requests apply to general contact and all contact pair interactions in a model by default in Abaqus/Standard. Options to limit an output request to certain interactions are discussed below.

CONTACT OUTPUT, NSET=node_set_name

Step module: field or history output request editor: Domain: Interaction: contact_interaction_name

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

Step module: field or history output request editor: Domain: Interaction: contact_interaction_name

CONTACT OUTPUT, SURFACE=surface_name

Field output requests apply to general contact and all contact pair interactions in a model by default in Abaqus/Explicit. Options to limit a surface field output request to certain interactions are discussed below.

CONTACT OUTPUT, CPSET=contact_pair_set_name

Step module: field output request editor: Domain: Interaction: contact_interaction_name

CONTACT OUTPUT, GENERAL CONTACT

CONTACT OUTPUT, SURFACE=surface_name

CONTACT OUTPUT, SURFACE=first_surface_name, 
SECOND SURFACE=second_surface_name

You must specify an interaction to which a surface history output request applies with one of the methods discussed below.

CONTACT OUTPUT, CPSET=contact_pair_set_name

Step module: history output request editor: Domain: Interaction: contact_interaction_name

CONTACT OUTPUT, SURFACE=surface_name

Step module: history output request editor: Domain: General contact surface: surface_name

CONTACT OUTPUT, SURFACE=first_surface_name, 
SECOND SURFACE=second_surface_name

CONTACT OUTPUT, NSET=node_set_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 1. 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

Step module: field or history output request editor: Preselected defaults or 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

Step module: history output request editor: Select from list below 

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

Step module: history output request editor: Preselected defaults or All

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.

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