Solution dialog box (Abaqus)

General

Analysis Type	Specifies the type of analysis to perform.Select Structural or Axisymmetric Structural to perform one the following types of analyses:Static stress (General or Perturbation)Eigenvalue buckling predictionNatural frequency extractionComplex eigenvalue extractionTransient modal dynamicResponse spectrumViscoDirect cyclicImplicit dynamicSteady-state modal dynamicYou use the Step option in the Solution Step dialog box to specify which of these types of analysis to perform in a step.Select Thermal or Axisymmetric Thermal to perform a steady-state or transient heat transfer analysis.Select Dynamic Explicit or Axisymmetric Dynamic Explicit to perform a dynamic explicit analysis.Select Coupled Thermal-Structural to perform a coupled thermal-structural analysis, which can be transient or steady-state.Select Dynamic Coupled Thermal-Structural to perform a dynamic coupled thermal-structural analysis. Select Modal Flexible Body to perform a flexible body modal analysis. For more information, see Abaqus analysis types.
2D Solid Option	Identifies the plane on which you can create axisymmetric elements. Also identifies the axis of rotation for axisymmetric elements.The solution uses the 2D Solid Option value that was set for the associated FEM file. You cannot modify this value.
Solution Type	Displays the current solution type.
Automatically Create Step or Subcase	Lets you select to automatically create a solution step of the selected type.
Transient Integration Options
These options are available only when:The Simulation includes a defined condition sequence.You select New Solution from Condition Sequence.Axisymmetric thermal analysis is not supported.Transient Integration Options define how condition sequence time history information is translated into time-dependent boundary conditions and time-step settings.
Option	Specifies the integration method:Step sizeIntegrates time history data based on the specified step duration in seconds, minutes, or hours.Number of time stepsIntegrates time history data based on the total number of time steps in the condition sequence.
Step size	Specifies the duration of a single time step.
Number of steps	Specifies the total number of time steps in the transient solution.
General Analysis/Heat Transfer/Dynamic Explicit/Coupled Temperature Displacement/Dynamic Coupled Temperature-Displacement/Modal Flexible Body options
Description	Lets you specify a description for the solution.The software uses any text that you enter in the Description box in the Solution dialog box as the *HEADING text. If you leave the Description box blank, the software does not include the *HEADING keyword in the Abaqus input file when you export or solve the solution.
Default Temperature	Lets you specify the default temperature to apply at nodes. This option corresponds to the Abaqus *INITIAL CONDITIONS, TYPE=TEMPERATURE keyword.Note: If you define initial conditions for temperatures using the Initial Conditions constraint, they override the default temperature you set here.
Run Job in Foreground	Lets you control whether the Abaqus job runs in the foreground or background:Select the Run Job in Foreground check box to run the Abaqus job in the foreground so the software is unavailable during the solve. Clear the Run Job in Foreground check box to run in the background so you can use this software while the solve is running. You can even close the software.

Eigenvalue Extraction

Modal Flexible Body solution options
Number of Desired Modes	Sets the number of eigenmodes to be extracted.
Frequency – Lower Limit	Sets the minimum frequency of interest, in cycles per time. If you do not enter a value, no minimum is set.
Frequency – Upper Limit	Sets the maximum frequency of interest, in cycles per time. If you do not enter a value, no maximum is set.

Output Controls

Modal Flexible Body solution options
Frequency Extraction Output
U - Displacement	Outputs all physical displacement components, including rotations at nodes with rotational degrees of freedom. Un displacement component (n =1, 2, 3) and URn rotation component (n =1, 2, 3).
RF - Reaction Forces and Moments	Outputs all components of reaction forces, including components of reaction moments at nodes with rotational degrees of freedom (conjugate to prescribed displacements and rotations). RFn reaction force component n (n =1, 2, 3) and RMn reaction moment component n (n =1, 2, 3).
S - Stress	Outputs all stress components. Sij-component of stress (i ≤ j ≤ 3).
E - Strain	Outputs all strain components. Eij-component of strain (i ≤ j≤ 3).
STH - Section Thickness	Outputs section thickness.
Matrix Substructure Output
Lets you output a substructure's recovery matrix, reduced stiffness matrix, mass matrix, load case vectors, and the gravity load vectors to a file. You must select to output a mass matrix file to use the results in a flexible body solution in Motion.
Recovery Matrix	Outputs a recovery matrix.
Reduced Stiffness Matrix	Outputs a reduced stiffness matrix.
Mass Matrix	Outputs a mass matrix.
Load Case Vectors	Outputs load case vectors.
Gravity Vectors	Outputs gravity vectors.

Optional Controls

Printout for the Analysis Input Files Processor
Contact Constraint Information	Prints detailed information about the contact constraints generated by the contact pair definition data to the .dat file.This option corresponds to CONTACT parameter for the Abaqus *PREPRINT keyword.
Input File Echo	Prints an echo of the input file data in the .dat file.This option corresponds to ECHO parameter for the Abaqus *PREPRINT keyword.
History Definition Summary	Prints a summary of history data to the .dat file.This option corresponds to HISTORY parameter for the Abaqus *PREPRINT keyword.
Model Definition Summary	Prints a summary of the model definition data to the .dat file.This option corresponds to MODEL parameter for the Abaqus *PREPRINT keyword.
Parameter-Free Input File Information	Prints the modified version of the original input file that is free of input model parametrization to the .dat file.This option corresponds to PARSUBSTITUTION parameter for the Abaqus *PREPRINT keyword.
Input Parameter Information	Prints the parameters used for model parametrization and their values to the .dat file.This option corresponds to PARVALUES parameter for the Abaqus *PREPRINT keyword.
Format of the Results FileAppears for Structural analyses.
Results File Output Format	Specifies the format of the results file (FIL), either ASCII or binary. If you do not specify a format, the results file is output in binary format. This option corresponds to the ASCII and BINARY parameters of the Abaqus *FILE FORMAT keyword.
Zero-increment Results File Output	Writes the results file (FIL) output at the beginning of a step (the zero increment). If you do not select zero increment, the results are written at the increment specified in the output request of the step.This option corresponds to the ZERO INCREMENT parameter of the Abaqus *FILE FORMAT keyword.

Physical Constants

Export Physical Constants	Appears for Structural, Axisymmetric Structural, Dynamic Explicit, and Axisymmetric Dynamic Explicit analyses:Select User-specified to specify individual constants to include in the Abaqus input file.Select As required by the solution to include only the constants that are necessary for the specific solution. For example, if your solution uses a creep material with the Hyperbolic Law formulation, the software includes the Absolute Zero constant in the Abaqus input file.For Thermal and Axisymmetric Thermal analyses, you can select which individual constants to write out to the input file. By default, the software writes out all three constants.
Absolute Zero	For Structural, Axisymmetric, Dynamic Explicit, and Axisymmetric Dynamic Explicit analyses, appears when you set Export Physical Constants to User-specified. Always appears for all other analyses.Includes the Absolute Zero constant in your solution. This option corresponds to the ABSOLUTE ZERO parameter for the Abaqus *PHYSICAL CONSTANTS keyword.The value that the software exports for the Absolute Zero constant is hard coded and depends on your current units system. For example, in the SI m units system, the software exports a value of -273.15.
Universal Gas Constant	For Structural, Axisymmetric, Dynamic Explicit, and Axisymmetric Dynamic Explicit analyses, appears when you set Export Physical Constants to User-specified. Always appears for all other analyses.Includes the Universal Gas Constant in your solution. This option corresponds to the UNIVERSAL GAS CONSTANT parameter for the Abaqus *PHYSICAL CONSTANTS keyword.The value that the software exports for the Universal Gas Constant constant is hard coded and depends on your current units system. For example, in the SI m units system, the software exports a value of -8.31434.
Stefan Boltzmann	For Structural, Axisymmetric, Dynamic Explicit, and Axisymmetric Dynamic Explicit analyses, appears when you set Export Physical Constants to User-specified. Always appears for all other analyses.Includes the Stefan Boltzmann constant in your solution. This option corresponds to the STEFAN BOLTZMANN parameter for the Abaqus *PHYSICAL CONSTANTS keyword.The value that the software exports for the Stefan Boltzmann constant is hard coded and depends on your current units system. For example, in the SI m units system, the software exports a value of 5.669E-8.

Solution Control

Contact Property Assignments	Appears for Structural and Dynamic Explicit analyses only. Lets you create a Contact Property Assignment modeling object to include in the solution.For more information, see Defining contact properties for general contacts (Abaqus).

Initial Conditions

Default Temperature	Appears for Thermal analyses only. Lets you specify the default temperature to apply at nodes. This option corresponds to the Abaqus *INITIAL CONDITIONS, TYPE=TEMPERATURE keyword.Note: If you define initial conditions for temperatures using the Initial Conditions constraint, they override the default temperature you set here.

User Defined Text

User Defined Text in Model	Lets you select a User Defined Text modeling object to include in the solution. For more information, see Customizing a Nastran input file with user defined text.

Restart

Restart Parameters
Define Job Name Of The Run To Be Read	Select the Define Job Name Of The Run To Be Read check box to indicate that the restart is a continuation of a previous analysis.Clear the Define Job Name Of The Run To Be Read check box to indicate that the restart is not a continuation of a previous analysis.
Job Name	Appears when the Define Job Name Of The Run To Be Read check box is selected. Lets you specify the name of the analysis to restart.
Restart At The Last Available Step Found	Appears when the Define Job Name Of The Run To Be Read check box is selected. Select the Restart At The Last Available Step Found check box to have Abaqus restart the analysis at the last available step it finds.Clear the Restart At The Last Available Step Found check box to specify the step number from which to restart the analysis.
Restart From Step Number	Appears when the Define Job Name Of The Run To Be Read check box is selected and the Restart At The Last Available Step Found check box is cleared. Lets you specify the number of the step from which to restart the analysis.
Restart From Last Available Increment	Appears when the Define Job Name Of The Run To Be Read check box is selected. Select the Restart From Last Available Increment check box to have Abaqus restart the analysis at the end of the step you specified in the Restart From Step Number box.Clear the Restart From Last Available Increment check box to specify the increment number within the step you specified in Restart From Step Number box after which to restart the analysis.
Restart from Increment Number	Appears when the Define Job Name Of The Run To Be Read check box is selected and the Restart From Last Available Increment check box is cleared.Lets you specify the increment number within the step that you specified in the Restart from Step Number box. Abaqus resumes the analysis after this increment.
Complete Current Step	Appears when the Define Job Name Of The Run To Be Read check box is selected. Select the Complete Current Step check box to terminate the current step in the solution that you are restarting.Clear the Complete Current Step check box to have Abaqus continue the analysis to complete the current step as it is defined in the solution that you are restarting.
Restart Analysis Option	Appears when the Define Job Name Of The Run To Be Read check box is selected. Select Continue With Additional Steps to specify the step number to use as the starting point for additional loading history data. Select Continue An Interrupted Run to continue the analysis without any additional history data.
Supply History Data From Solution Step Number	Appears when the Define Job Name Of The Run To Be Read check box is selected and Restart Analysis Option is set to Continue With Additional Steps. Lets you specify the step number to use as the starting point for additional loading history data.

Submodel

Submodel	Lets you type the name of the results (.fil) or database (.odb) file containing the global results to drive the submodel analysis. For more information, see Submodel constraint (Abaqus).
Name of the Global Model Results	Type the name of the results (.fil) or database (.odb) file containing the global results to drive the submodel analysis.

How do I

Create or modify a solution

Create or modify a solution step or subcase

Learn more

Solutions

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Solution dialog box (Abaqus), 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 } });