Abaqus Structural, Explicit, Thermal, and Thermal-Structural Output Requests dialog box

Common options for Structural, Dynamic Explicit, Axisymmetric Dynamic Explicit, Thermal, Coupled Thermal-Structural, and Dynamic Coupled Thermal-Structural Requests

Name and Description
Name	Defines the name of the modeling object.
Label	Sets a unique numerical identifier for the modeling object.This label also appears in the Modeling Objects Manager dialog box, and you can filter the objects listed in that dialog box by their label.
Description	Enter a brief description or click to open a text editor where you can enter a longer description.
ODB File Output Control
Written into ODB File	Controls whether the software creates an output database (.odb) file during the analysis. This option corresponds to the *OUTPUT keyword in Abaqus.
Field/History option	If you select Written Into ODB File, this option lets you specify whether you want to output the data as field-type, history-type, or field and history-type output.
Output Variables	Available when the Written into ODB File check box is selected.Controls the variables the software outputs to the ODB file.Select All to have the software output all variables that are applicable to the current type of Solution Step and material type.Select Preselect to have the software output the default output variables for the current type of Solution Step.Select Select From List to have the software output the variables that you select on the output tabs at the bottom of the dialog box.
The following options are available for Thermal analyses with any type of output selected.
Field Output Frequency Domain	Controls the output frequency to the database (.odb) file.FrequencyControls the frequency of element output. Select Frequency and then from the Output Frequency list that appears, select the default frequency or a selected frequency.Number of IntervalsLets you specify the frequency, in increments, at which the software outputs results.Time Interval SizeLets you specify the time intervals at which the software should output results.Time PointsLets you specify a time points modeling object that defines the time points at which output is to be written.
Output Frequency	Available when Field Output Frequency Domain is set to Frequency.Controls the frequency of element output.Specified FrequencyLets you specify the frequency to be output.Default FrequencyLets you specify that the default frequency be output.
Specify Frequency	Available when Output Frequency is set to Specified Frequency. Lets you specify the frequency, in increments, at which the software outputs results. If you specify a frequency of 0, the software suppresses the output and only outputs the variables in the last increment of the step.This option corresponds to the *EL PRINT, FREQUENCY=n syntax in Abaqus.
Specify Intervals	Available when Field Output Frequency Domain is set to Specify Intervals. Type the number of intervals during the step at which the file output states are to be written. The software always writes the results at the beginning of the step. For example, if you specify 10, the software writes 11 results states consisting of the values at the beginning of the step and the values at the end of 10 intervals throughout the step. The value of this parameter must be a positive integer.
Time Interval	Available when Field Output Frequency Domain is set to Time Interval Size. Type the time intervals at which the software should output results.
Time Marks	Appears when Field Output Frequency Domain is set to any option but Frequency. To write the results at the increment ending immediately after the time specified in the Specify Number of Intervals box, select the Time Marks check box. To write results at the exact times entered in the Specify Number of Intervals box, clear the Time Marks check box. You cannot select Time Marks if you selected Fixed Time Incrementation or Direct User Control when defining the step in the Solution Step dialog box. This option corresponds to the TIME MARKS= syntax in Abaqus.For more information, see Solution Step dialog box (Abaqus), Explicit Dynamic Step Setup page.
The following options are available for explicit analyses with field-type output selected.
Field Output Frequency Domain	Controls the output frequency to the ODB file:Select Number of Intervals and then in the Specify Intervals box that appears, type the number of intervals at which the software should output results. Select Time Interval Size and then in the Time Interval box that appears, type the time intervals at which the software should output results. Select Time Points and then set Specify Time Points to the time points modeling object that defines the time points at which output is to be written. To create a time points modeling object, click Create Modeling Object .For more information, see Time Points dialog box (Abaqus).
Time Marks	Appears when Field Output Frequency Domain is set to Number of Intervals or Time Points.Select the Time Marks check box to write the results at the increment ending immediately after the time specified in Specify Number of Intervals. Clear the Time Marks check box to write results at the exact times entered in Specify Number of Intervals. You cannot select Time Marks if you selected Fixed Time Incrementation or Direct User Control when defining the step in the Solution Step dialog box. This option corresponds to the TIME MARKS= syntax in Abaqus.For more information, see Solution Step dialog box (Abaqus), Explicit Dynamic Step Setup page.
Include Element Material Directions	Controls whether to write the element material directions to the output database.Set to YES (the default) to write the element material directions to the output database. Set to NO to not write the element material directions to the output database. This option corresponds to the DIRECTION= syntax in Abaqus.
Elemental Result Position	Controls from where on the element, the element values are being written:Set to Integration Points (the default) if values are being written at the integration points at which the variables are actually calculated.Set to Centroidal if values are being written at the centroid of the element (the centroid of the reference surface of a shell element, the midpoint between the end nodes in a beam element). Set to Nodes if the values being written are extrapolated to the nodes of each element in the set but not averaged at the nodes.This option corresponds to the POSITION= syntax in Abaqus.
Section Points for Shell or Beam Elements	For beams, shells, or layered solid elements, the software provides output at the default section points. Select this option to specify output points other than the default section points.To select the sections, click Specify and then in the Specify Section Points box, type the section points. Click to select the section points.To accept the default output points, select Default.
Element/Node Field Output Variables	Controls the variables the software outputs to the ODB file.To have the software output all variables that are applicable to the current type of Solution Step and material type, select All.To have the software output the default output variables for the current type of Solution Step, select Preselect.To have the software output the variables that you select on the output tabs at the bottom of the dialog box, select Select From List.
The following options are available for explicit analyses with history-type output selected.
History Output Frequency Domain	Controls the output frequency of history-type output to the ODB file.Select Number of Increments and then in the Specify Increments box that appears, type the number of increments at which the software should output results. Select Time Interval Size and then in the Time Interval box that appears, type the time intervals at which the software should output results.
Vector-Values Nodal Variables In Global Directions	Controls whether to write vector-valued nodal variables in the local or global directions.Select the Vector-Values Nodal Variables In Global Directions check box to write vector-valued nodal variables in the local directions. Clear the Vector-Values Nodal Variables In Global Directions check box to write vector-valued nodal variables in the global directions.
Section Points For Layered Shell Elements	For beams, shells, or layered solid elements, the software provides output at the default section points. Select this option to specify output points other than the default section points.To select the sections, click Specify and then in the Specify Section Points, type the section points. Click to select the section points.To accept the default output points, select Default.
Element/Node History Output Variables	Controls the variables the software outputs to the ODB file.Select All to have the software output all variables that are applicable to the current type of Solution Step and material type.Select Preselect to have the software output the default output variables for the current type of Solution Step.Select Select from List to have Abaqus output the variables that you select on the output tabs at the bottom of the dialog box.
FIL/DAT file output control
Written into FIL file	Controls whether the software creates a results (FIL) file during the analysis.
Written into DAT file	Controls whether the software creates a data (DAT) file that contains printed output of the model during the analysis.
Summary	Available when the Written into DAT file check box is selected.Controls whether the software prints summaries of element variables in the data file. If you select Yes, the software prints a summary of the minimum and maximum values at the end of each column in an output table. The software also prints the locations of the minimum and maximum values.This option corresponds to the *EL PRINT, SUMMARY=YES or NO syntax in Abaqus.
Total	Available when the Written into DAT file check box is selected.Controls whether the software prints the sum (total) of each column in an output data to the data file. You can use totals, for example, to obtain a sum of all the energies in a set of elements.This option corresponds to the *EL PRINT, TOTALS=YES or NO syntax in Abaqus.
RES/FIL File Output Control
Written Into RES/FIL File	Controls whether the software creates a restart (RES) and binary result (FIL) file during the analysis. To select additional options to control the information (element output, nodal output, and/or energy output requests) the software reports to the files, select the Written Into RES/FIL File check box.To only report the defaults, clear the Written Into RES/FIL File check box.This option corresponds to the *FILE OUTPUT keyword in Abaqus.
Specify Number of Intervals	Type the number of intervals during the step at which the file output states are to be written. The software always writes the results at the beginning of the step. For example, if you specify 10, the software writes 11 results states consisting of the values at the beginning of the step and the values at the end of 10 intervals throughout the step. The value of this parameter must be a positive integer.
Time Marks	To write the results at the increment ending immediately after the time specified in Specify Number of Intervals, select the Time Marks check box. To write results at the exact times entered in Specify Number of Intervals, clear the Time Marks check box. You cannot select Time Marks if you selected Fixed Time Incrementation or Direct User Control when defining the step in the Solution Step dialog box. This option corresponds to the TIME MARKS= syntax in Abaqus.For more information, see Solution Step dialog box (Abaqus), Explicit Dynamic Step Setup page.
Element/Node Output Variables	The only available option is Select from List, which instructs the software to output the variables that you select on the output tabs at the bottom of the dialog box.
Element Position File Output Control
Elemental Result Position	Controls the position at which the software lists the output. These options correspond to the *EL PRINT, POSITION= syntax in Abaqus.Integration PointsProvides the output variables at the integration points where they are calculated.CentroidalProvides the output variables at the centroid of each element.Average at NodesExtrapolates the output variables to the nodes. With this option, the software averages the output variables over all the elements that contribute to each node.NodesProvides the output variables at the nodes of each element.
Frequency Output Control
Output Frequency	Controls the frequency of element output.Specified FrequencyLets you specify the frequency to be output.Default FrequencyLets you specify that the default frequency be output.
Specify Frequency	Available if you set Output Frequency to Specified Frequency. Lets you specify the frequency, in increments, at which the software outputs results. If you specify a frequency of 0, the software suppresses the output and only outputs the variables in the last increment of the step.This option corresponds to the *EL PRINT, FREQUENCY=n syntax in Abaqus.
MSG/STA file output control
Written into MSG/STA file	Controls whether the software creates a message (MSG) and status (STA) file during the analysis. If you select the Written into MSG/STA file check box, you can then select additional options to control the information the software reports to the message file.
Adaptive Mesh	Reports details about adaptive mesh smoothing, including the magnitude of the maximum displacement as well as the labels of the nodes at which geometric feature changes occur.This option corresponds to the*PRINT, ADAPTIVE MESH=YES or NO syntax in Abaqus.
Contact	Reports information about the contact conditions during iteration, such as which points are contacting or separating.This option corresponds to the *PRINT, CONTACT=YES or NO syntax in Abaqus.
Model Change	Reports details about model change operations (removal and reactivation) at the start of a step.This option corresponds to the *PRINT, MODEL CHANGE=YES or NO syntax in Abaqus.
Plasticity	Reports the labels and integration points of elements for which the plasticity algorithms fail to converge during an iteration.This option corresponds to the *PRINT, PLASTICITY=YES or NO syntax in Abaqus.
Residual	Reports the equilibrium residuals during equilibrium iterations.This option corresponds to the *PRINT, RESIDUAL=YES or NO syntax in Abaqus.
Solve	Reports the number of equations being solved and the amount of memory required for each iteration.This option corresponds to the *PRINT, SOLVE=YES or NO syntax in Abaqus.
Global/Local Directions
Include Local Coordinate Directions When Available	Lets you request that the local coordinate directions be written to the results file if component output is requested for any variable.This option corresponds to the *EL FILE, DIRECTIONS=YES syntax in Abaqus.
Output at layered section points
All Section Points (ODB + Field Output)	Available for all solutions except Axisymmetric Dynamic Explicit. Available when the Written Into ODB File check box is selected and Field/History is set to Field or Field And History.For 2D solid elements, select to output results at all section points. This option corresponds to the *OUTPUT FIELD keyword and the ALLSECTIONPTS parameter of the *ELEMENT OUTPUT Abaqus keyword.
Output at Layered Section Points	For beams, shells, or layered solid elements, the software provides output at the default section points. Select this option to specify output points other than the default section points.Note: In Dynamic Explicit analyses, you can set Output at Layered Section Points to either Use Defaults or Specify with Specify Section Points set to ALL. They are equivalent because, by default, the software provides output at all section points in Abaqus Dynamic Explicit solutions.
Specify Section Points	Available if you set Output at Layered Section Points to Specify. Click to select the section points at which you want the software to provide the output.
Entity
Entity	Lets you control the entities on which the software lists results.ALLLists results on all nodes and elements.GROUP/NODE GROUP/ELEMENT GROUPLists results on the elements or nodes in a selected group.Tip: If you have many groups defined, click More Options and use the Filter by Name option to filter the list of groups, or use the Find option to search for a group. Note: In the Forces/Reaction group, for the following node-based and element-based output components, be sure to define and select groups with the appropriate content, either nodes or elements. Node-based: RF, RT, RM, TF, and CF Element-based: NFORC, P, SF, TRSHR, and TRNORWhen you create the groups, be sure to set the Type Filter selection (Elements and/or Nodes) so the groups contain the correct entities and are consistent. Geometry-based groups are not supported for output requests.

Stresses

Output Variables
S - Stress components and invariants	Lists all stress components.
All stress components	Appears when the S - Stress components and invariants check box is selected. Requests all stress components be output. Clear the check box to select an individual stress component.
S11 - Component of stress S22 - Component of stress S33 - Component of stress S12 - Component of stress S13 - Component of stress S23 - Component of stress	Available when the All stress components check box is cleared. Selects a component of stress to be output.
MISESMAX - Maximum mises equivalent stress	Lists the maximum Mises equivalent stress.
TSHR - Transverse shear stress (for thick shells)	Lists all transverse shear stress components for thick shell elements, such as S3R, S4R, S8R, and S8RT.
CTSHR - Transverse shear stress in stacked continuum shells	Lists transverse shear stress components for stacked continuum shell elements (SC6R and SC8R).
CFAILURE - All failure measure components	Lists all failure measure components for stress.
VS - Stress in the elastic-viscous network	Lists the stress in the elastic-viscous network.
PS - Stress in the elastic-plastic network	Lists the stress in the plastic-viscous network.

Strains

Output Variables
E - Total strain components	Lists all strain components. For more information, see Total (integrated) strain in the Conventions section of the Abaqus Analysis User's Guide.
All strain components	Appears when the E - Total strain components check box is selected. Requests all strain components be output. Clear the check box to select an individual strain component.
E11 - Component of strain E22 - Component of strain E33 - Component of strain E12 - Component of strain E13 - Component of strain E23 - Component of strain	Available when the All strain components check box is cleared. Selects a component of strain to be output. Note: Strain components Eij are not valid for .fil and field .odb output files. If you select these components for output to .fil and field .odb files, the software writes E (all strain components) instead so post-processing can extract and display Eij.
VE - Viscous strain in the elastic-viscous network	Lists the viscous strain in the elastic-viscous network.
PE - Plastic strain components	Lists the components of plastic strain.
EE - Elastic strain components	Lists the components of elastic strain.
IE - Inelastic strain components	Lists the components of inelastic strain.
THE - Thermal strain components	Lists the components of thermal strain.
NE - Nominal strain components	For large-strain shell, membrane, and solid elements, lists the components of nominal strain. For more information, see Nominal strain in the Conventions section of the Abaqus Analysis User's Guide.
LE - Logarithmic strain components	For large-strain shell, membrane, and solid elements, lists the components of logarithmic strain. For more information, see Logarithmic strain in the Conventions section of the Abaqus Analysis User's Guide.
SE - Section strains and curvatures	Lists the section strains and curvatures. See Elements in the Abaqus Analysis User's Guide for a list of which section strains are available for each beam or shell element type.
VEEQ - Equivalent viscous strain in the elastic-viscous network	Lists the equivalent viscous strain in the elastic-viscous network
PEEQ - Equivalent plastic strain	Lists the equivalent plastic strain in the elastic-plastic network.
PEEQMAX - Maximum equivalent plastic strain	Lists the maximum equivalent plastic strain value (PEEQ) among all section points. For a shell element, PEEQMAX represents the maximum PEEQ value among all the section points in the layer.For a beam element, PEEQMAX is the maximum PEEQ among all the section points in the cross-section.For a solid element, PEEQMAX represents the PEEQ at the integration points.
PEMAG - Plastic strain magnitude	Lists the magnitude of plastic strain.
CEEQ - Equivalent Creep Strain	Lists the equivalent creep strain.If you request the output variable for a specific group, the group must be an element-based group. Tip: When you create a group, set the filter to Element to create an element-based group for output request.

Displacement/Velocity/Acceleration

Output Variables
U - Translations and rotations	Lists all physical displacement components, including rotations at nodes with rotational degrees of freedom
All translations and rotations	Appears when the U - Translations and rotations check box is selected. Requests all physical displacement components be output. Clear the check box to select individual components.
U1 - Displacement component U2 - Displacement component U3 - Displacement component UR1 - Rotation component UR2 - Rotation component UR3 - Rotation component	Available when the All translations and rotations check box is cleared. Selects a physical displacement component to be output.
UT - Translations	Lists all translational displacement components.
UR - Rotations	Lists all rotational displacement components.
V - Translational and rotational velocities	Lists all velocity components, including rotational velocities at nodes with rotational degrees of freedom.
All velocity components	Appears when the V - Translational and rotational velocities check box is selected. Requests all velocity components be output. Clear the check box to select individual components.
V1 - Translational velocity component V2 - Translational velocity component V3 - Translational velocity component VR1 - Rotational velocity component VR2 - Rotational velocity component VR3 - Rotational velocity component	Available when the All velocity components check box is cleared. Selects a velocity component to be output.
VT - Translational velocities	Lists all translational velocity components.
VR - Rotational velocities	Lists all rotational velocity components.
A - Translational and rotational accelerations	Lists all acceleration components.
All acceleration components	Appears when the A - Translational and rotational accelerations check box is selected. Requests all acceleration components be output. Clear the check box to select individual components.
A1 - Translational acceleration component A2 - Translational acceleration component A3 - Translational acceleration component AR1 - Rotational acceleration component AR2 - Rotational acceleration component FR3 - Rotational acceleration component	Available when the All acceleration components check box is cleared. Selects an acceleration component to be output.
AT - Translational accelerations	Lists all translational acceleration components.
AR - Rotational accelerations	Lists all rotational acceleration components.

Forces/Reactions

Output Variables
NFORC - Forces at the nodes	Lists nodal forces due to element stress.
P - Distributed pressure load	Lists uniformly distributed pressure load on element faces.Note: The P component is only available for output database field (.odb) files. If you select to output P to .fil or history .odb files, the software issues a warning and does not output the component.
All components of reaction forces and moments	Appears when the RF - Reaction forces and moments check box is cleared. Requests all components of reaction forces be output. Clear to select individual components.
RF - Reaction forces and moments	Lists all components of reaction forces, including components of reaction moments at nodes with rotational degrees of freedom (conjugate to prescribed displacements and rotations).
RF1 - Reaction force component RF2 - Reaction force component RF3 - Reaction force component RM1 - Reaction moment component RM2 - Reaction moment component RM3 - Reaction moment component	Available when the All components of reaction forces and moments check box is cleared. Selects a component of reaction forces to be output.
RT - Reaction forces	Lists all reaction force components.
RM - Reaction moments	Lists all reaction moment components.
SF - Section forces and moments	Lists all section forces and moments. See Elements in the Abaqus Analysis User's Guide for a list of which section forces are available for each beam or shell element type.
TF - Total forces and moments	Lists all components of total forces, including components of total moments at nodes with rotational degrees of freedom. Total force is the sum of the reaction force and point loads.
All components of total forces and moments	Appears when the TF - Total forces and moments check box is cleared. Requests all components of total forces or total moments be output. Clear to select individual components.
TF1 - Total force component TF2 - Total force component TF3 - Total force component TM1 - Total moment component TM2 - Total moment component TM3 - Total moment component	Available when the All components of total forces and moments check box is cleared. Selects a component of total forces or total moments to be output.
TRSHR - Shear traction vector	Lists the shear component (component along face tangent) of a traction load on element faces.
TRNOR - Normal component of traction vector	Lists the normal component (component along face normal) of traction load on element faces.
CF - Concentrated forces and moments	Lists all components of point loads and concentrated moments.
All components of point loads and concentrated moments	Appears when the CF - Concentrated forces and moments check box is cleared. Requests all components of point loads or point moments be output. Clear to select individual components.
CF1 - Point load component CF2 - Point load component CF3 - Point load component CM1 - Point moment component CM2 - Point moment component CM3 - Point moment component	Available when the All components of point loads and concentrated moments check box is cleared. Selects a component of point load or point moment to be output.

Contact

Entity
Entity	Lets you control the entities on which the software writes the results for contact analyses. ALLIncludes output for the entire contact domain.SURFACELimits surface field output requests to a single surface in the general contact domain.NSETAppears for Structural analyses.Lists results for a subset of slave nodes.SURFACE AND NSETAppears for Structural analyses.Includes output for the master and slave surfaces and a subset of slave nodes.CONTACT PAIR SETAppears for Dynamic Explicit analyses.Sets the contact pairs for which surface field output is desired. By default, the output requests apply to all contact pair interactions in the model. GENERAL CONTACT DOMAINAppears for Dynamic Explicit analyses.Limits surface field output requests to apply only to the general contact.
Surface/Second Surface (Optional)	Available for Dynamic Explicit analyses when Entity is set to SURFACE.Lets you specify the surfaces for which to generate output. Either select an existing contact region that contains the surfaces or click Create Region to create a new region.
Master /Slave	Available for Structural analyses when Entity is set to SURFACE or SURFACE and NSET.Lets you specify the surfaces for which to generate output. Either select an existing contact region that contains the surfaces or click Create Region to create a new region.
Nset	Available when Entity is set to NSET or SURFACE and NSET.Lets you specify the group that contains the slave nodes for which to generate output.
Contact Pair	Available when Entity is set to Contact Pair Set.Specifies the contact pair for which to generate output. Select an existing contact pair or click Create Modeling Object to create a new contact pair.
Output Variables
CSTRESS - Contact stresses	Lists contact pressure (CPRESS) and frictional shear stress (CSHEAR). CSHEAR is not available for general contact analyses
All CSTRESS components	Appears when the CSTRESS - Contact stresses check box is cleared. Requests all components of contact stress. Clear to select individual components.
CPRESS - Contact pressure (DAT file only) CSHEAR1 - Contact frictional shear stress (DAT file only) CSHEAR2 - Contact frictional stress (DAT file only)	Available when the All CSTRESS components check box is cleared. Selects a component of CSTRESS to be output. Note: Components CPRESS, CSHEAR1, and CSHEAR2 are only valid for .dat files. Therefore, if you request any of these components as output to an .odb or .fil file, the software outputs the variable CSTRESS so post-processing can extract and display CPRESS, CSHEAR1, or CSHEAR2 output results.
CDSTRESS - Contact damping stresses	Lists viscous pressure (CDPRESS) and viscous shear stresses (CDSHEAR).
CDISP - Contact displacements	Lists contact opening (COPEN) and relative tangential motions (CSLIP).
All CDISP components	Select to request all CDISP components or clear to select individual components.
COPEN - Contact opening (DAT file only) CSLIP1 - Relative tangential motion (DAT file only) CSLIP2 - Relative tangential motion (DAT file only)	Available when the All CDISP components check box is cleared. Select a component of CDISP to output. Note: Components COPEN, CSLIP1, and CSLIP2 are only valid for .dat files. Therefore, if you request any of these components as output to an .odb or .fil file, the software outputs the variable CDISP so post-processing can extract and display COPEN, CSLIP1, or CSLIP2 output results.To view COPEN, CSLIP1, or CSLIP2 output results in post-processing, you need to select the customer default option Read Unknown Results.
CFORCE - Contact forces	Lists contact normal force (CNORMF) and frictional shear force (CSHEARF).
CNAREA - Contact area associated with each node in contact	Lists the total area in contact.
CSTATUS - Contact status	Lists the status of contact in the model.
FSLIP	Appears for Dynamic Explicit analyses. Lists the length of contact slip path at slave nodes during contact (FSLIPEQ) and, in some cases, components of net contact slip in local tangent directions (FSLIP1 and FSLIP2).
FSLIPR - Contact slip rate	Appears for Dynamic Explicit analyses. Lists the magnitude of the contact slip rate at slave nodes during contact (FSLIPR) and in some cases components of contact slip rate in local tangent directions (FSLIPR1 and FSLIPR2).
PPRESS - Fluid pressure load	Lists fluid pressure load on element faces (the results of the Pressure Penetration simulation object).

Energy

Output Variables
ENER - All energy magnitudes	Lists all energy densities.
ELEN - All energy magnitudes in the element	Lists energy magnitudes in the element. None of the energies are available in mode-based procedures
ALLSD – Energy dissipated by automatic stabilization	Available if you select the Written into ODB file check box in the ODB file output control options and then select History from the Field/History Option list.Calculates the energy that is dissipated by automatic stabilization for a selected group of elements or the entire model. This calculation includes both volumetric static stabilization and the automatic approach of contact pairs.
ALLSE – Recoverable energy strain	Available if you select the Written into ODB file check box in the ODB file output control options and then select History from the Field/History Option list.Calculates the recoverable energy strain of a selected group of elements or the entire model.
ETOTAL – Total energy balance	Available if you select the Written into ODB file check box in the ODB file output control options and then select History from the Field/History Option list.Calculates the total energy balance of the entire model.

Thermal/Thermal (Elemental)/Thermal (Nodal)

Output Variables
NT – Nodal temperature	Outputs all temperature values at a node.Note: This output variable is available for both structural and thermal analyses.
RFL – Nodal reaction flux	Outputs the total flux at the node, including flux convected through the node in convection elements, and excluding external fluxes.
TEMP – Element temperature	Outputs all temperature values at an element.
HFL – Element heat flux	Outputs the current magnitude and components of the heat flux per unit area vector for an element.

Contact (Thermal analyses)

Output Variables
HFLA – HFL multiplied by the nodal area	Outputs HFL multiplied by the nodal area.
HTL – Time integrated HFL	Outputs time-integrated HFL, which is heat flux per unit area leaving the slave surface.
HTLA – Time integrated HFLA	Outputs time-integrated HFLA, which is HFL multiplied by the nodal area.

Cavity Radiation

Output Variables
FTEMP - Facet temperature	Outputs facet temperature.
RADFL – Radiation flux per unit area	Outputs radiation flux per unit area.
RADFLA – Radiation flux over the facet	Outputs radiation flux over the face.

Solution-Dependent State Variable

Output Variables
SDV	Outputs the solution-dependent state variables.
STATUS	Available for Abaqus Structural, Dynamic Explicit, Coupled Thermal-Structural, and Dynamic Coupled Thermal-Structural analyses and for all Abaqus results files.Outputs the status of elements. The status of an element is 1.0 if the element is active; 0.0 if the element is not. Tip: To output the status of all elements, set Entity to ALL. To output only a subset of elements, set Entity to GROUP and select a group of elements.

Geometric Quantities

Output Variables
IVOL - Integration point volume	Lists the section point volume of beams and shells.If you request the output variable for a specific group, the group must be an element-based group. Tip: When you create a group, set the filter to Element to create an element-based group for output request.

Connector Element Output Variables

Available for all solutions except Thermal, Thermal-Structural, and Dynamic Coupled Thermal-Structural.

Output Variables
CTF - Connector total forces and moments	Lists all components of connector total force and moment.
All components of connector total forces and moments	Appears when the CTF - Connector total forces and moments check box is cleared. Requests all components of connector total force and moment be output. Clear to select individual components.
CTF1 - Connector total force component CTF2 - Connector total force component CTF3 - Connector total force component CTM1 - Connector total moment component CTM2 - Connector total moment component CTM3 - Connector total moment component	Available when the All components of connector total forces and moments check box is cleared. Selects a component of total force or moment to be output. Note: The total force and moment components are only valid for .dat files. Therefore, if you request any of these components as output to an .odb or .fil file, the software outputs the variables CTF and CU.
CEF - Connector elastic forces and moments	Requests connector elastic forces and moments.
CU - Connector relative displacements and rotations	Lists the components of connector relative displacement and rotation in all directions.
All components of connector relative displacements and rotations	Appears when the CU - Connector relative displacements and rotations check box is cleared. Requests all components of connector relative displacement and rotation be output. Clear to select individual components.
CU1 - Connector relative displacement CU2 - Connector relative displacement CU3 - Connector relative displacement CUR1 - Connector relative rotation CUR2 - Connector relative rotation CUR3 - Connector relative rotation	Available when the All components of connector relative displacements and rotations check box is cleared. Selects a component of relative displacement or rotation in the n direction (1, 2, or 3) to be output.
CUE - Connector elastic displacements and rotations	Requests connector elastic displacements and rotations in all directions.
CUP - Connector plastic displacements and rotations	Requests connector plastic displacements and rotations in all directions.

Learn more

Requesting output for Abaqus analyses

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Abaqus Structural, Explicit, Thermal, and Thermal-Structural Output Requests dialog box, Simcenter 3D 2021.1 Series

© 2020 Siemens

window.mainLanguage="en_US"

window.delivId=""

window.projectId=""

MathJax.Hub.Config({ TeX: { extensions: ["autoload-all.js"] }, tex2jax: { displayMath: [ ] }, "SVG": { scale: 125 } });