CategoryOutput variables
Whole element variablesEDT, EMSF, ELEDEN, ESEDEN, EPDDEN, ECDDEN, EVDDEN, EASEDEN, EIHEDEN, EDMDDEN, ELEN, ELSE, ELCD, ELPD, ELVD, ELASE, ELIHE, ELDMD, ELDC, STATUS
Nodal output variablesNT, COORD
Table 4.1.3–4 Output variables that cannot be digitally filtered or modified with bounding values.
CategoryOutput variables
Cracking model quantitiesCRACK
Element face variablesSTAGP, TRNOR, TRSHR
Whole element variablesGRAV, BF, SBF, P
Nodal output variablesCF
# 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 output database. Modal output is available only as history output. # Controlling the frequency of output The frequency of modal output is controlled as described above in “Controlling the output frequency in Abaqus/Standard.” # Requesting output 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. Input File Usage: \*MODAL OUTPUT, VARIABLE=ALL Abaqus/CAE Usage: Step module: history output request editor: All # Surface output in Abaqus/Standard and Abaqus/Explicit You can write variables associated with surfaces in contact, coupled thermal-electrical-structural (Abaqus/Standard only), coupled temperature-displacement (Abaqus/Standard only), coupled thermal-electrical, and crack propagation problems to the output database. Multiple output requests can be used to customize requests among interactions, surfaces, or node sets. For surface variables associated with cavity radiation, see “Cavity radiation output in Abaqus/Standard” below. Use element output requests (see “Element output”) to obtain database output for contact elements (such as gap elements; see “Gap contact elements,” Section 40.2.1). In Abaqus/Standard contact history output cannot be saved in a linear perturbation step with frequency extraction. Displacement nodal output is generated automatically in Abaqus/Explicit when requesting surface output. # Selecting the surface output variables 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. Input File Usage: \*CONTACT OUTPUT list of output variables Abaqus/CAE Usage: Step module: field or history output request editor: Select from list below # Limiting the extent of a surface output request in Abaqus/Standard 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. Limiting output to a node set in Abaqus/Standard You can limit a surface output request to apply to a subset of surface nodes involved in contact pairs or general contact in Abaqus/Standard. Input File Usage: \*CONTACT OUTPUT, NSET=node\_set\_name Abaqus/CAE Usage: Step module: field or history output request editor: Domain: Interaction: contact\_interaction\_name Limiting output for contact pairs based on slave and master surface names in Abaqus/Standard You can limit output to certain contact pairs based on surface names. If you specify both the slave and master surface names, the output request is limited to a specific contact pair. If you specify the slave surface but not the master surface, output is written for all contact pairs that involve the specified slave surface. If you also specify a node set, the applicability of an output request is further limited (i.e., the output request will generate output only for certain nodes of a certain contact pair (or pairs). Output requests with a specific slave and/or master surface role specified will not generate output for general contact. Input File Usage: \*CONTACT OUTPUT, MASTER=master, SLAVE=slave, NSET=node\_set\_name Abaqus/CAE Usage: Step module: field or history output request editor: Domain: Interaction: contact\_interaction\_name Limiting output for cracked surfaces in enriched elements based on surface name in Abaqus/Standard You can limit output requests to certain cracked surfaces in enriched elements based on surface names. Input File Usage: \*CONTACT OUTPUT, SURFACE=surface\_name Abaqus/CAE Usage: You cannot limit surface field output for cracked surfaces in enriched elements in Abaqus/CAE. # Limiting the extent of a surface field output request in Abaqus/Explicit 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. Limiting surface field output to a contact pair set in Abaqus/Explicit In Abaqus/Explicit you can select the contact pairs for which surface field 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. Input File Usage: Use the following option to request surface field output for a particular contact pair set: \*CONTACT OUTPUT, CPSET=contact\_pair\_set\_name Abaqus/CAE Usage: Step module: field output request editor: Domain: Interaction: contact\_interaction\_name Limiting surface field output to general contact in Abaqus/Explicit You can limit surface field output requests to apply only to general contact in Abaqus/Explicit, but you cannot further limit this output to a subset of the general contact domain. Input File Usage: \*CONTACT OUTPUT, GENERAL CONTACT Abaqus/CAE Usage: You cannot limit surface field output to general contact in Abaqus/CAE. Limiting surface field output to a single surface in Abaqus/Explicit You can limit surface field output requests to a single surface in the general contact domain in Abaqus/Explicit. The contact output for the specified surface will include all the contributions from other contact surfaces interacting with the surface. This type of output should not be used for surfaces involving beam, truss, or pipe elements. Input File Usage: \*CONTACT OUTPUT, SURFACE=surface\_name Abaqus/CAE Usage: You cannot limit a single surface output to general contact in Abaqus/CAE. Limiting surface field output to pairwise surfaces in Abaqus/Explicit You can specify a pair of surfaces in the general contact domain in Abaqus/Explicit for which the interactions on one surface due to the contact with another surface will be output. This type of output cannot be used for surfaces involving Eulerian regions and should not be used for surfaces involving beam, truss, or pipe elements. Input File Usage: \*CONTACT OUTPUT, SURFACE=first\_surface\_name, SECOND SURFACE=second\_surface\_name Abaqus/CAE Usage: You cannot limit pairwise surface output to general contact in Abaqus/CAE. # Specifying surface history output regions in Abaqus/Explicit You must specify an interaction to which a surface history output request applies with one of the methods discussed below. Specifying surface history output by contact pair set in Abaqus/Explicit In Abaqus/Explicit you can select the contact pairs for which surface history 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. Input File Usage: Use the following option to request surface history output for a particular contact pair: \*CONTACT OUTPUT, CPSET=contact\_pair\_set\_name Abaqus/CAE Usage: Step module: history output request editor: Domain: Interaction: contact\_interaction\_name Specifying whole surface history output in Abaqus/Explicit You can specify a surface in the general contact domain for which whole surface contact force resultants will be output. Whole surface contact force resultants for a surface in the general contact domain are available only as history output. Input File Usage: \*CONTACT OUTPUT, SURFACE=surface\_name Abaqus/CAE Usage: Step module: history output request editor: Domain: General contact surface: surface\_name Specifying pairwise surface history output in Abaqus/Explicit You can specify a pair of surfaces in the general contact domain for which the resultant contact forces on one surface due to the contact with another surface will be output. The contact force resultants in this case consider only the contact interactions between the two specified surfaces. This type of output cannot be requested for surfaces involving Eulerian regions. Input File Usage: \*CONTACT OUTPUT, SURFACE=first\_surface\_name, SECOND SURFACE=second\_surface\_name Abaqus/CAE Usage: You cannot request surface history output for a pair of surfaces in Abaqus/CAE. Specifying surface history output by fastened node set in Abaqus/Explicit You can select a fastened node set for which bond history output is desired: Input File Usage: Use the following option to request surface history output for a particular fastened node set: \*CONTACT OUTPUT, NSET=node\_set\_name Abaqus/CAE Usage: You cannot request surface history output for a particular fastened node set in Abaqus/CAE. # Controlling the output frequency The frequency of surface output is controlled as described above in “Controlling the output frequency.” # Requesting preselected output You can request the preselected, procedure-specific surface output variables described in Table 4.1.3–1. In this case you can specify additional variables as part of the output request. Alternatively, you can request all surface variables applicable to the current procedure. In this case any additional variables you specify are ignored. Input File Usage: Use the following option to request the preselected surface output variables: \*CONTACT OUTPUT, VARIABLE=PRESELECT Use the following option to request all applicable surface output variables: \*CONTACT OUTPUT, VARIABLE=ALL Abaqus/CAE Usage: Step module: field or history output request editor: Preselected defaults or All # Surface output in Abaqus/CFD You can write field and history output variables associated with surfaces in an Abaqus/CFD analysis to the output database. # Selecting the surface output variables The surface variables that can be written to the output database are listed in the “Surface variables” section of “Abaqus/CFD output variable identifiers,” Section 4.2.3. Input File Usage: \*SURFACE OUTPUT, SURFACE=surface\_set\_name list of output variables Abaqus/CAE Usage: You cannot request surface output in Abaqus/CAE. # Controlling the output frequency The frequency of surface output is controlled as described above in “Controlling the output frequency.” # Time incrementation output in Abaqus/Explicit You can output incrementation variables for an Abaqus/Explicit analysis to the output database. Incrementation output is available only as history output. # Selecting the incrementation output variables 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. Input File Usage: \*INCREMENTATION OUTPUT list of output variables Abaqus/CAE Usage: Step module: history output request editor: Select from list below # Controlling the output frequency The frequency of incrementation output is controlled as described above in “Controlling the output frequency for history output in Abaqus/Explicit.” # Requesting preselected output 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. Input File Usage: Use the following option to request the preselected incrementation output variables: \*INCREMENTATION OUTPUT, VARIABLE=PRESELECT Use the following option to request all applicable incrementation output variables: \*INCREMENTATION OUTPUT, VARIABLE=ALL Abaqus/CAE Usage: Step module: history output request editor: Preselected defaults or All # Cavity radiation output in Abaqus/Standard You can request that cavity-, element-, or surface-based output such as radiation fluxes, view factor totals for a facet, and facet temperatures from an Abaqus/Standard analysis be written to the output database. The output request can be repeated as often as necessary to define output for different variables, different cavities, different element sets, different surfaces, etc. # Selecting the radiation output variables 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. Input File Usage: \*RADIATION OUTPUT list of output variables Abaqus/CAE Usage: Cavity radiation output requests are not supported in Abaqus/CAE. # Selecting the region of the model for which radiation output is required 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. Input File Usage: Use one of the following options: \*RADIATION OUTPUT, CAVITY=cavity\_name \*RADIATION OUTPUT, ELSET=element\_set\_name \*RADIATION OUTPUT, SURFACE=surface\_name Abaqus/CAE Usage: Cavity radiation output requests are not supported in Abaqus/CAE. # Controlling the output frequency The frequency of radiation output is controlled as described above in “Controlling the output frequency.” # Requesting output You can request all radiation variables applicable to the current procedure. In this case any additional variables you specify are ignored. Input File Usage: \*RADIATION OUTPUT, VARIABLE=ALL Abaqus/CAE Usage: Cavity radiation output requests are not supported in Abaqus/CAE. # Examples The examples that follow illustrate how to request multiple types of output over multiple steps in both Abaqus/Standard and Abaqus/Explicit. # Abaqus/Standard example 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. ```asm *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 ``` # Abaqus/Explicit example 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. ```txt *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 ```