<!-- source-page: 811 -->

# 5.1 Accessing the results file

• “Accessing the results file: overview,” Section 5.1.1   
• “Results file output format,” Section 5.1.2   
• “Accessing the results file information,” Section 5.1.3   
• “Utility routines for accessing the results file,” Section 5.1.4

<!-- source-page: 812 -->

<!-- source-page: 813 -->

# 5.1.1 ACCESSING THE RESULTS FILE: OVERVIEW

# Writing information to the results file

The Abaqus results file is the medium through which analysis results can be carried over into other software, such as postprocessing programs. The following types of output can be written to the results file:

• element output, nodal output, energy output, modal output, contact surface output, and section output (see “Output to the data and results files,” Section 4.1.2)   
• element matrix output (see “Element matrix output in Abaqus/Standard” in “Output,” Section 4.1.1)   
• substructure matrix output (see “Writing the recovery matrix, reduced stiffness matrix, mass matrix, load case vectors, and gravity vectors to a file” in “Defining substructures,” Section 10.1.2)   
• cavity radiation view factor matrices (see “Writing the view factor matrices to the results file” in “Cavity radiation,” Section 41.1.1)

“Output,” Section 4.1.1, describes the general format of the results file.

An Abaqus model can be defined in terms of an assembly of part instances (see “Defining an assembly,” Section 2.10.1). However, the results file is not organized by part; it contains internal node and element numbers (see “Output,” Section 4.1.1). A map between the original numbers and part instance names and the internal numbers is written to the data file.

# Accessing information in the results file

This chapter contains technical descriptions of the results file and is intended to be read by users or programmers who need to write programs that use the results file.

• “Results file output format,” Section 5.1.2, describes the format of the individual records in the results file.   
• “Accessing the results file information,” Section 5.1.3, describes the subroutine calls required to read the file output, contains an example of a program written to use the Abaqus results file, and shows how you can write (or modify) a results file using the Abaqus file format.   
• “Utility routines for accessing the results file,” Section 5.1.4, describes the utility subroutines that can be used to access the results file.

<!-- source-page: 814 -->

<!-- source-page: 815 -->

# 5.1.2 RESULTS FILE OUTPUT FORMAT

Products: Abaqus/Standard Abaqus/Explicit

# References

• “Accessing the results file: overview,” Section 5.1.1   
• “Abaqus/Standard output variable identifiers,” Section 4.2.1   
• “Abaqus/Explicit output variable identifiers,” Section 4.2.2

# Overview

This section describes the format of the individual records in the Abaqus results file. Where applicable, the output variable identifier used in writing a given value to the file is printed below the corresponding record type description. Records that are available only in Abaqus/Standard are designated with an (S) ; records that are available only in Abaqus/Explicit are designated with an (E) . The record key for a particular record may differ between Abaqus/Standard and Abaqus/Explicit.

# Record format

The results file is written as a sequential file. Each record has the following format:

<table><tr><td>Location</td><td>Length</td><td>Description</td></tr><tr><td>1</td><td>1</td><td>Record length (NW)</td></tr><tr><td>2</td><td>1</td><td>Record type key</td></tr><tr><td>3, 4...</td><td>(NW - 2)</td><td>Attributes</td></tr></table>

All words in the results file are of the same length, whether they contain integer, floating point number, or character string data. The word length is that of a double precision floating point number (8 bytes).

The attributes in a given record may depend on the element type being considered. For example, the stress components associated with three-dimensional shell elements are $\sigma _ { 1 1 } , \sigma _ { 2 2 }$ , and $\sigma _ { 1 2 }$ (in local directions), while those associated with three-dimensional solids are $\sigma _ { x x } , \sigma _ { y y } , \sigma _ { z z } , \sigma _ { x y } , \sigma _ { x z }$ , and $\sigma _ { y z }$ (in global directions if no local orientation is specified). Thus, care must be used in interpreting the data when postprocessing the file output. Refer to Part VI, “Elements,” for a definition of the ordering of element-dependent attributes.

In steady-state dynamic analyses, complex values are stored as the real components followed by the imaginary components. For example, the stress components associated with three-dimensional shell elements are $\Re ( \sigma _ { 1 1 } ) , \Re ( \sigma _ { 2 2 } )$ , and $\Re ( \sigma _ { 1 2 } )$ followed by ${ \mathfrak { I } } ( \sigma _ { 1 1 } ) , { \mathfrak { I } } ( \sigma _ { 2 2 } )$ , and $\Im ( \sigma _ { 1 2 } )$ .

In models that are defined in terms of an assembly of part instances, the results file contains internal (global) node and element numbers, as explained in “Output,” Section 4.1.1. Part and assembly records are not included in the results file.

<!-- source-page: 816 -->

# Local coordinate system

If the components of an element quantity are in local directions, a record of type 85 defining these directions is generated for each point at which component output is requested if the local coordinate directions were requested in Abaqus/Standard (see “Output of local directions to the results file” in “Output to the data and results files,” Section 4.1.2) and automatically in Abaqus/Explicit. The local coordinate system may be inherent to the element, as is the case in shells and membranes, or may have been defined by a local orientation (see “Orientations,” Section 2.2.5).

For shell elements a direction record is written for every material point in the section for which component output is requested, and a separate direction record is written for section forces and section strains. For geometrically nonlinear analysis in Abaqus/Standard the record contains the current, updated directions, except for small-strain shells, in which case the original directions are given. Direction output is not provided for trusses, two-dimensional beams, axisymmetric shells or membranes, or for values averaged at nodes.

# Label record

Some record types include labels, such as element and node set names, written in A8 format. If a label exceeds 8 characters, an integer identifier will be written instead. This identifier can then be used to cross-reference the actual label stored in 10A8 format on record type 1940.

Records written for any file output request 

<table><tr><td>Record key</td><td>Record type</td><td>Attributes</td></tr><tr><td>1900</td><td>Element definitions</td><td>1. Element number.2. Element type (characters, A8 format, left justified).3. First node on the element.4. Second node on the element.5. Etc.</td></tr><tr><td> $1990^{(S)}$ </td><td>Element definition continuation</td><td>1. Node on the element in the previous 1900 record.2. Etc.</td></tr></table>

In Abaqus/Explicit quadrilateral/brick elements that are degenerate (i.e., possessing identical nodes) are written out in record 1900 as corresponding triangular/tetrahedral/wedge elements. For example, a CPE4R element with two identical nodes is written as a CPE3 element, and a C3D8R element with identical third and fourth nodes and identical seventh and eighth nodes is written as a C3D6 element.

1901 Node definitions

1. Node number.   
2. First coordinate.   
3. Second coordinate.   
4. Etc.

<!-- source-page: 817 -->

# Record Record type Attributes key

Record key 1902 (below) defines the location of each active degree of freedom. For example, if the model contains only two-dimensional beam elements, the only active degrees of freedom are 1, 2, and 6. Therefore, this record would have the attributes $( 1 , 2 , 0 , 0 , 0 , 3 )$ , meaning that degree of freedom 1 $( u _ { x } )$ is the first active variable at each node; degree of freedom $2 \left( u _ { y } \right)$ is the second active variable at each node; degrees of freedom 3, 4, and 5 are not active in the model; and degree of freedom 6 is the third active variable at each node.

<table><tr><td>1902</td><td>Active degrees of freedom</td><td>1. Location in nodal arrays of degree of freedom 1 (0 if DOF 1 is not active in the model).2. Location in nodal arrays of degree of freedom 2 (0 if DOF 2 is not active in the model).3. Etc.</td></tr><tr><td> $1910^{(S)}$ </td><td>Substructure path</td><td>1. 0 substructure enter record; 1 substructure leave record.2. Element number on usage level.3. Substructure type identifier (Zn).4. Element number at the previous level if it is not the usage level.5. Etc.</td></tr><tr><td>1911</td><td>Output request definition</td><td>1. Flag for element-based output (0), nodal output (1), modal output (2), or element set energy output (3).2. Set name (node or element set) used in the request (A8 format). This attribute is blank if no set was specified.3. Element type (only for element output, A8 format).</td></tr><tr><td>1921</td><td>Abaqus release, etc.</td><td>1. Abaqus release number (A8 format).2. Date (2A8 format).3. Date cont&#x27;d.4. Time (A8 format).5. Number of elements in the model.6. Number of nodes in the model.7. Typical element length in the model.</td></tr><tr><td>1922</td><td>Heading</td><td>1. Attributes 1–10. The heading entered as the first data line of the *HEADING option (A8 format). Equivalent to the job description in Abaqus/CAE.</td></tr></table>

<!-- source-page: 818 -->

<table><tr><td>Record key</td><td>Record type</td><td>Attributes</td></tr><tr><td>1931</td><td>Node set</td><td>1. Node set name (A8 format). In Abaqus/Explicit only node sets defined as part of the model definition are written.2. First node in the node set.3. Second node in the node set.4. Etc.</td></tr><tr><td>1932</td><td>Node set continuation</td><td>1. Node number in the node set of the previous 1931 record.2. Etc.</td></tr><tr><td>1933</td><td>Element set</td><td>1. Element set name (A8 format). In Abaqus/Explicit only element sets defined as part of the model definition are written.2. First element in the element set.3. Second element in the element set.4. Etc.</td></tr><tr><td>1934</td><td>Element set continuation</td><td>1. Element number in the element set of the previous 1933 record.2. Etc.</td></tr><tr><td>1940</td><td>Label cross-reference</td><td>1. Integer reference.2. Label (10A8 format).</td></tr></table>

Record written once per eigenvalue in natural frequency extraction 

<table><tr><td>Record key</td><td>Record type</td><td>Attributes</td></tr><tr><td> $1980^{(S)}$ </td><td>Modal</td><td>1. Eigenvalue number.2. Eigenvalue.3. Generalized mass.4. Composite damping.5. Participation factor for degree of freedom 1.6. Effective mass for degree of freedom 1.7. Participation factor for degree of freedom 2.8. Effective mass for degree of freedom 2.9. Etc.</td></tr></table>

Any nodal or element data after this record refer to the eigenvector, until a new record key 1980 or a record key 2001 is encountered. Eigenvalue output for substructures (see “Writing the recovery matrix, reduced stiffness matrix, mass matrix, load case vectors, and gravity vectors to a file” in “Defining substructures,” Section 10.1.2) also uses these records to divide up elemental and nodal results. This record is written if

<!-- source-page: 819 -->

# Record Record type Attributes key

there are any results file output requests for an eigenvalue buckling prediction or eigenfrequency extraction step. The generalized mass, etc. are not written for an eigenvalue buckling prediction step. This record is not written for a complex eigenfrequency extraction step.

Records written once per increment 

<table><tr><td>Record key</td><td>Record type</td><td>Attributes</td></tr><tr><td>2000</td><td>Increment start record</td><td>1. Total time.2. Step time.3. Maximum creep strain-rate ratio (control of solution-dependent amplitude) in Abaqus/Standard; currently not used in Abaqus/Explicit.4. Solution-dependent amplitude in Abaqus/Standard; currently not used in Abaqus/Explicit.5. Procedure type: gives a key to the step type. See Table 5.1.2-1 at the end of this section.6. Step number.7. Increment number.8. Linear perturbation flag in Abaqus/Standard: 0 if general step, 1 if linear perturbation step; currently not used in Abaqus/Explicit.9. Load proportionality factor: nonzero only in static Riks steps; currently not used in Abaqus/Explicit.10. Frequency (cycles/time) in a steady-state dynamic response analysis or steady-state transport angular velocity (rad/time) in a steady-state transport analysis; currently not used in Abaqus/Explicit.11. Time increment.12. Attributes 12-21. The step subheading entered as the first data line of the *STEP option (A8 format). Equivalent to the step description in Abaqus/CAE.</td></tr></table>

The following record is written once per increment, after all data records have been written for that increment.

2001 Increment end record

1. No attributes.

<!-- source-page: 820 -->

# Record Record type key

# Attributes

Note: When binary format is used, the results file is written in blocks of 512 words for each increment. If there are fewer than 512 words in the last block of the current increment, record 2001 has zeros appended to it so that the total length of the block is 512. Hence, the length of record 2001 is 2 + the number of zeros appended. For an ASCII format results file record 2001 is extended to complete an 80 character logical record, and a logical record of 80 blank characters is added after this record. See “Accessing the results file information,” Section 5.1.3.

# Records written for any element file output request

These records contain data about element variables at integration points within the elements, at the centroid of elements, or at the nodes of an element.

# Record Record type key

1 Element header record

# Attributes

1. Element number or the node number if the subsequent records contain nodal averaged element values.   
2. Integration point number if the subsequent records contain integration point data. Node number if the subsequent records contain data at the nodes of the element. Integration plane number if the subsequent records contain centroidal values for CAXA and SAXA elements. 0 if the subsequent records contain centroidal values or nodal averaged values.   
3. Section point number if this is a shell, beam, or layered solid element and the subsequent records contain data at a section point through the thickness. 0 for continuum elements and for section values in beams and shell elements.   
4. Location identification. 0 if the subsequent records contain data at an integration point; 1 if the subsequent records contain values at the centroid of the element; 2 if the subsequent records contain data at the nodes of the element; 3 if the subsequent records contain data associated with rebar within an element; 4 if the subsequent records contain nodal averaged values; 5 if the subsequent records contain values associated with the whole element.
