<!-- source-page: 631 -->

# Selecting the nodal output variables

The nodal variables that can be written to the data and results files are defined in the “Nodal variables” portion of “Abaqus/Standard output variable identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2.

Abaqus allows only complete sets of basic variables (for example, all of the displacement components) to be written to the results file. Individual variables (such as a particular displacement component) cannot be selected and must be obtained by postprocessing.

# Selecting the nodes for which output is required

You can specify the node set for which output is being requested. If you do not specify a node set, the output will be printed for all nodes in the model.

```txt
Input File Usage: Use either of the following options:
*NODE PRINT, NSET=node_set_name
*NODE FILE, NSET=node_set_name 
```

# Requesting summaries in the Abaqus/Standard data file

By default in Abaqus/Standard, summaries of nodal variables are printed in the data file. A summary of the maximum and minimum values is printed at the end of each column in an output table. The locations of the maximum and minimum values are also printed. You can choose to suppress this summary.

Input File Usage: \*NODE PRINT, SUMMARY=YES or NO

# Requesting totals in the Abaqus/Standard data file

In Abaqus/Standard you can print the sum (total) of each column in an output table to the data file. Totals can be used, for example, to sum reaction forces at the nodes. By default, these totals are suppressed.

Input File Usage: \*NODE PRINT, TOTALS=YES or NO

# Controlling the frequency of output

In Abaqus/Standard you can control the frequency of nodal output by specifying the output frequency in increments. Unless a frequency of zero is specified to suppress output, the variables will always be output at the last increment of the step.

In Abaqus/Explicit the frequency of nodal output is controlled as described in “Output frequency” above.

Input File Usage: Use either of the following options in Abaqus/Standard:

```txt
*NODE PRINT, FREQUENCY=n
*NODE FILE, FREQUENCY=n 
```

# Specifying the directions for nodal output

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.

<!-- source-page: 632 -->

In Abaqus/Standard components of nodal variables such as reaction forces are output 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. The local directions defined by the nodal transformation cannot be written to the results file.

The data in the Abaqus/Explicit selected results file are always output in the global directions, even if a local coordinate system has been defined at a node.

# Obtaining nodal output in the global directions

In Abaqus/Standard you can request vector-valued nodal variables in the global directions, which is the default for nodal output requests to the results file since most postprocessors assume that components are given in the global system.

Input File Usage: Use either of the following options:

\*NODE PRINT, GLOBAL=YES

\*NODE FILE, GLOBAL=YES

Obtaining nodal output in the local directions defined by nodal transformations

In Abaqus/Standard you can request vector-valued nodal variables in the local directions defined by nodal transformations, which is the default for nodal output requests to the data file.

Input File Usage: Use either of the following options:

\*NODE PRINT, GLOBAL=NO

\*NODE FILE, GLOBAL=NO

# Controlling the output during eigenvalue extraction

You can control nodal output during natural frequency extraction, complex eigenvalue extraction, and eigenvalue buckling analysis by specifying the first and last mode numbers for which output is required, as described above for element output.

Input File Usage: Use either of the following options:

$\ast \mathrm { N O D E ~ P R I N T , ~ M O D E } { = } m , \mathrm { L A S T ~ M O D E } { = } n$

\*NODE FILE, MODE=m, LAST MODE=n

# Abaqus/Standard data file format

In Abaqus/Standard the printed output of variables is arranged in tables by node set in the data file. For nodal variables each row of a table corresponds to an individual node.

Each table is defined by a data line of the nodal output request, which specifies the variables to appear in that table. There is no limit to the number of tables that can be defined. The first column of each table is the node number. You choose the variables to appear in the remaining columns; up to nine variables (columns) can appear in a table. If all of the entries in a row are zero, the row is not printed. Displacement, velocity, and acceleration components less than a relative tolerance (equal to 100 times the machine precision times the current maximum value in the model) are treated as zero.

<!-- source-page: 633 -->

# Results file format

There is no header or direction record for nodes, so it makes little difference whether items are requested on a single line or multiple lines. In Abaqus/Standard if all results in a record are zero, the record is not written to the results file.

# Default nodal output

If you do not specify a nodal output request to the results file in a step (or in any previous step of the analysis), no nodal output will be written to the results file; similarly if you do not specify a nodal output request to the data file (available only in Abaqus/Standard) in a step (or in any previous step of the analysis), no nodal output will be written to the data file.

# Total energy output

You can output summaries of the energy content of the model to the Abaqus/Standard data (.dat) file, the Abaqus/Standard results (.fil) file, or the Abaqus/Explicit selected results (.sel) file. Energy output requests are not available for the following procedures:

• “Eigenvalue buckling prediction,” Section 6.2.3   
• “Natural frequency extraction,” Section 6.3.5   
• “Complex eigenvalue extraction,” Section 6.3.6

Energy output requests remain in effect for subsequent steps. Detailed energy density output is available by using element output requests (see “Element output”).

In Abaqus/Explicit the energy output is written to the selected results (.sel) file, which must be converted to the results (.fil) file as explained above.

# Input File Usage:

Use the following option to output summaries of the energy content to the Abaqus/Standard data file:

\*ENERGY PRINT

Use the following option to output summaries of the energy content to the Abaqus/Standard results file or the Abaqus/Explicit selected results file:

\*ENERGY FILE

# External work calculation due to concentrated follower forces

Abaqus/Standard may generate inaccurate external work (ALLWK) in the presence of a concentrated follower load that rotates with time (see “Specifying concentrated follower forces” in “Concentrated loads,” Section 34.4.2). This problem may occur in both static and implicit dynamic analyses and may result in an inaccurate total energy (ETOTAL) history output. Other results (displacements, stresses, strains, etc.) are not affected. The inaccuracy is due to the fact that the increment of work is calculated using the direction of the concentrated load at the end of the increment instead of using an average load over the increment.

<!-- source-page: 634 -->

# Selecting the energy output variables

When energy output is requested, all of the total energy quantities listed in “Abaqus/Standard output variable identifiers,” Section 4.2.1, or “Abaqus/Explicit output variable identifiers,” Section 4.2.2, are output; the variables cannot be selected individually.

# Selecting the element set for which total energy output is required

In Abaqus/Standard 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,” Section 6.3.7   
• “Mode-based steady-state dynamic analysis,” Section 6.3.8   
• “Response spectrum analysis,” Section 6.3.10   
• “Random response analysis,” Section 6.3.11

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.

In Abaqus/Explicit you cannot specify selected element sets for an energy output request; the total energies for the whole model will always be output.

Input File Usage: Use one of the following options in Abaqus/Standard:

\*ENERGY PRINT, ELSET=element\_set\_name

\*ENERGY FILE, ELSET=element\_set\_name

# Controlling the frequency of output

In Abaqus/Standard you can control the frequency of energy output by specifying the output frequency in increments. Unless a frequency of zero is specified to suppress output, the variables will always be output at the last increment of the step.

In Abaqus/Explicit the frequency of energy output is controlled as described in “Output frequency” above.

Input File Usage: Use either of the following options in Abaqus/Standard:

\*ENERGY PRINT, FREQUENCY=n

\*ENERGY FILE, FREQUENCY=n

# Default energy output

Energy output requests must be included for total energy output to be written to the data and results files; no default output is provided.

<!-- source-page: 635 -->

# Modal output from Abaqus/Standard

You can output generalized coordinate (modal amplitude and phase) values during modal dynamic procedures (see “Dynamic analysis procedures: overview,” Section 6.3.1, for an overview of the modal dynamic procedures available in Abaqus/Standard) to the data (.dat) file or results (.fil) file.

You can also request that eigenvalues be written to the results file during “Eigenvalue buckling prediction,” Section 6.2.3, or “Natural frequency extraction,” Section 6.3.5. The eigenvalues are always written to the results file when element or nodal output to the results file is requested; however, modal output requests allow you to write the eigenvalues to the results file without requesting any additional output.

Input File Usage: Use the following option to output modal variables to the Abaqus/Standard data file:

\*MODAL PRINT

Use the following option to output modal variables to the Abaqus/Standard results file:

\*MODAL FILE

# Selecting the modal output variables

The modal variables that can be written to the data and results files are defined in the “Modal variables” portion of “Abaqus/Standard output variable identifiers,” Section 4.2.1.

# Controlling the frequency of output

You can control the frequency of modal output by specifying the output frequency in increments. Unless a frequency of zero is specified to suppress output, the variables will always be output at the last increment of the step.

Input File Usage: Use either of the following options:

\*MODAL PRINT, FREQUENCY=n

\*MODAL FILE, FREQUENCY=n

# Default modal output

Modal output requests must be included for modal results to be written to the data and results files; no default output is provided.

# Surface output from Abaqus/Standard

In Abaqus/Standard you can write variables associated with surfaces in contact, coupled temperaturedisplacement, coupled thermal-electrical-structural, coupled thermal-electrical, and crack propagation problems to the data and results files. The output requests can be repeated as often as necessary within a step to define output for different contact pairs and different types of surface variables.

<!-- source-page: 636 -->

See “Cavity radiation,” Section 41.1.1, for information on requesting output of surface variables associated with cavity radiation.

Use element output requests (see “Element output”) to obtain data and results file output for contact elements (such as slide line elements; see “Slide line contact elements,” Section 40.4.1).

# Selecting the surface output variables

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

• “Slave node” variables are associated with the integration points at which the material calculations are performed (for example, the contact stress).   
• “Whole surface” variables are attributes of an entire slave surface (for example, the total force due to contact pressure).

The surface variables that can be written to the data and results files are listed in the “Surface variables” portion of “Abaqus/Standard output variable identifiers,” Section 4.2.1.

# Selecting the contact pairs for which output is required

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 given for all contact pairs that involve the specified slave surface.

Input File Usage: Use either of the following options:

$$
\begin{array}{l} * \text { CONTACT   PRINT,   MASTER } = \text { master,   SLAVE } = \text { slave,   NSET } = \text { node\_set } \\ * \text { CONTACT   FILE,   MASTER } = \text { master,   SLAVE } = \text { slave,   NSET } = \text { node\_set } \\ \end{array}
$$

# Requesting summaries in the data file

By default, summaries of surface variables are printed in the data file. A summary of the maximum and minimum values is printed at the end of each column in an output table. The locations of the maximum and minimum values are also printed. You can choose to suppress this summary.

Input File Usage: \*CONTACT PRINT, SUMMARY=YES or NO

# Requesting totals in the data file

You can print the sum (total) of each column in an output table to the data file. By default, these totals are suppressed.

Input File Usage: \*CONTACT PRINT, TOTALS=YES or NO

# Controlling the frequency of output

You can control the frequency of surface output by specifying the output frequency in increments. Unless a frequency of zero is specified to suppress output, the variables will always be output at the last increment of the step.

<!-- source-page: 637 -->

Input File Usage: Use either of the following options:

\*CONTACT PRINT, FREQUENCY=n

\*CONTACT FILE, FREQUENCY=n

# Default surface output

Surface output requests must be included for surface variables associated with contact pairs to be written to the data and results files; no default output is provided.

If a surface output request is defined without any specified output variables, the following variables will be written to the data and results files by default:

• For contact analysis, contact pressure (CPRESS), frictional shear stresses (CSHEAR), contact opening (COPEN), and relative tangential motions (CSLIP); see “Defining contact pairs in Abaqus/Standard,” Section 36.3.1.   
• For heat transfer analysis, heat flux per unit area (HFL), heat flux (HFLA), time integrated HFL (HTL), and time integrated HFLA (HTLA); see “Thermal contact properties,” Section 37.2.1.   
• For coupled thermal-electrical analysis, HFL, HFLA, HTL, HTLA, electrical current per unit area (ECD), electrical current (ECDA), time integrated ECD (ECDT), and time integrated ECDA (ECDTA); see “Electrical contact properties,” Section 37.3.1.   
• For coupled pore fluid-mechanical analysis, CPRESS, CSHEAR, COPEN, CSLIP, pore fluid volume flux per unit area (PFL), pore fluid volume flux (PFLA), time integrated PFL (PTL), and time integrated PFLA (PTLA); see “Pore fluid contact properties,” Section 37.4.1.   
• For crack propagation analysis, there are no default output quantities; bond failure quantities must be requested explicitly; see “Crack propagation analysis,” Section 11.4.3.

# Data file format

Printed output of variables is arranged in tables. Each table is defined by a data line of the surface output request, which specifies the variables to appear in that table. Each table can contain only one type of output variable (slave node or whole surface). For example, output variables CSTRESS and CFN cannot be requested on the same data line. For the slave node type of output, each row of a table corresponds to a node on the slave surface. The rows that will appear in a particular table will be limited to the node set specified in the output request. The first column of each table defines the location (the node number). The remaining columns contain variables such as contact pressure, frictional shear stresses, contact opening, and relative tangential (slip) motions. For the whole surface type of output, each row of a table corresponds to an entire slave surface. If all of the variables in a row of a table are zero, the row is not printed.

If a contact output request refers to more than one contact pair, a separate table will be generated for each contact pair. All of the tables defined by the first data line of the output request will be printed, then all of the tables defined by the second line, etc.

# Results file format

A contact output request record (the type 1503 record described in “Results file output format,” Section 5.1.2) is created for each output request. For the slave node type of output, this record is

<!-- source-page: 638 -->

followed by several node header records, each of which contains a node on the slave surface. Each node header record is followed by records that contain output variables. The output will be limited to the node set specified in the output request. For the whole surface type of output, the type 1503 record is followed by only one type 1504 node header record with a node number zero. The node header record is followed by records containing the requested output variables.

If a contact output request refers to more than one contact pair, a separate contact output request record is generated for each contact pair.

# Section output from Abaqus/Standard

In Abaqus/Standard you can output accumulated quantities associated with user-defined sections (see “Abaqus/Standard output variable identifiers,” Section 4.2.1) for a particular step to the data or results file. This facility provides “free body diagram” output, allowing analyses of force flow through a redundant structure. The output requests can be repeated as often as necessary within a step to define output for different sections and different section output variables. You can assign a label to each output request that will be used to identify the output for the section. Section output is not available for eigenfrequency extraction, eigenvalue buckling prediction, complex eigenfrequency extraction, or linear dynamics procedures or in procedures using multiple load cases.

# Defining the surface section

Section output requests are available only for sections defined using element-based surfaces (see “Element-based surface definition,” Section 2.3.2). Consequently, the sections must be defined using faces of continuum elements although other types of elements (beams, membranes, shells, springs, dashpots, etc.) can be attached to the section.

Calculation of accumulated quantities on the section (such as the total force) involves nodal quantities associated with elements on one side of the section only. Therefore, the surface definition should use elements only from one side of the section (the “base elements,” as defined in “Prescribed assembly loads,” Section 34.5.1), thus precisely identifying the side from which accumulated quantities are computed.

Since the section usually cuts through the mesh in a typical section output request, automatic generation of the surface cannot be used. Specifying the element faces gives exact control over which element faces form the surface, which is essential when defining a cross-section through a solid body.

You must specify the name of the surface for which output is being requested.

Surfaces that are defined in a restart analysis can be used only for section output requests. The newly defined surface cannot be used for any other purpose (such as a contact pair or pre-tension section definition).

Input File Usage: Use either of the following options:

# Example

For example, the following input illustrates a typical section output request to the data file:

<!-- source-page: 639 -->

```txt
*HEADING
Section print example
...
*SURFACE, NAME=surface_name
Data lines that specify the elements and their associated faces to define the surface section
...
*STEP
...
*SECTION PRINT, NAME=section_name,
SURFACE=surface_name, ...
...
*END STEP 
```

Alternatively, if additional section output requests are needed after the analysis is completed, a restart analysis can be performed to request more output as shown in the following input:

```txt
*RESTART, READ, ...
...
*SURFACE, NAME=surface_name
Data lines that specify the elements and their associated faces to define the surface section
...
*STEP
...
*SECTION PRINT, NAME=section_name,
SURFACE=surface_name, ...
...
*END STEP 
```

# Selecting the coordinate system in which output is desired

You can specify the choice of coordinate system in which the section output is desired. By default, the components of vector quantities associated with the section are obtained with respect to the global system of coordinates. Alternatively, you can specify that output is desired in a local system as defined below.

Input File Usage: Use either of the following options:

```txt
*SECTION PRINT, NAME=section_name, SURFACE=surface_name, AXES=GLOBAL or LOCAL
*SECTION FILE, NAME=section_name, SURFACE=surface_name, AXES=GLOBAL or LOCAL 
```

# Defining a coordinate system local to the surface section

You can allow Abaqus/Standard to define the local system, or you can specify it directly.

<!-- source-page: 640 -->

# Default local system

The default local system is particularly useful when the section is flat or almost flat. While it can also be used in the case when the defined surface is curved, the default local system may be irrelevant for such problems.

The default system is defined by a straight line in two-dimensional and axisymmetric cases or by a plane in three-dimensional cases, fitted (in a least square sense) through the nodes belonging to the section. The anchor point (origin) of the local system is the centroid of the projection of the surface on the fitted line or plane. The local directions are given by the normal (1-direction) and the tangent direction (the 2-direction in two-dimensional and axisymmetric cases) or the tangent directions (the 2- and 3-directions in three-dimensional cases) to the fitted line or plane. When several straight lines or planes can be fit equally well between the nodes defining the section (for example, a closed circular or spherical surface), the original local directions will be parallel to the global axes.

The positive local 1-direction is selected such that it will form an acute angle with the average normal direction to the section, computed by averaging the positive normals to the element faces defining the section. If the average normal direction is zero (a closed surface), the 1-direction will form an acute angle with the global x-axis. If in two-dimensional or axisymmetric cases the 1-direction is within 0.1° of being normal to the global x-axis, it will form an acute angle with the global y-axis. In three-dimensional cases if the 1-direction is within 0.1° of being normal to the global X–Y plane, it will form an acute angle with the global z-axis.

In two-dimensional and axisymmetric cases the local 2-direction is obtained by rotating the local 1-direction counterclockwise by 90° about the anchor point. For three-dimensional situations the tangent directions of the surface are defined using the Abaqus conventions for local directions on surfaces in space (see “Conventions,” Section 1.2.2).

Input File Usage: Use either of the following options to use the default local coordinate system:

```txt
*SECTION PRINT, NAME=section_name, SURFACE=surface_name, AXES=LOCAL
*SECTION FILE, NAME=section_name, SURFACE=surface_name, AXES=LOCAL 
```

# User-specified local system

A user-specified local system is defined by specifying the origin and the directions of the axes. You can specify the origin (anchor point) by giving a node number or by specifying the coordinates of the anchor point.

In two-dimensional and axisymmetric cases the local 2-direction is defined by specifying either a predefined node number or the coordinates of a point (point a) on the local 2-direction. The local 1-direction is then obtained by rotating the local 2-axis clockwise by 90° about the anchor point (see Figure 4.1.2–1). If node numbers are used to define the anchor point or the local directions, they must be connected to the mesh.

In three-dimensional cases either two predefined nodes or the coordinates of two points can be used to specify the local directions. A rectangular Cartesian coordinate system is then defined by its origin (the anchor point) and these two points. The first point (point a) must lie on the local 2-direction, and
