Solution Step dialog box (Abaqus), General page

Properties
Description	Lets you specify a description for the step.	All step types
INC	Specifies the maximum number of increments in a single solution step.*STEP	All step types except perturbation
NLGEOM	Controls whether geometric nonlinearity should be accounted for in the current step.Select the NLGEOM check box to indicate that geometric nonlinearity should be accounted for during the step.Clear the NLGEOM check box to perform a geometrically linear analysis in the current step.This option corresponds to the NLGEOM parameter for the *STEP keyword.	All structural step types except perturbationDynamic Coupled Thermal-Stress
Unstable Problem Method	Lets you specify additional parameters to control the analysis.NoneAbaqus does not include the RIKS or STABILIZE parameters.RIKSUses the modified Riks method for proportional loading.This option corresponds to the RIKS parameter for the *STATIC keyword.STABILIZEUses automatic stabilization if you expect the problem to be unstable due to local instabilities.This option corresponds to the STABILIZE parameter for the *STATIC keyword.	General
Stabilization Factor	Appears when Unstable Problem Method is set to STABILIZE.Lets you specify a stabilization factor. The value you specify should be equal to the dissipated energy fraction of the automatic damping algorithm.See Solving nonlinear problems in the Abaqus Analysis User’s Guide for more information.	General
Max. Number of Increments Allowed	Lets you set the maximum number of increments in a step. The value is only an upper bound.	Steady-State Coupled Thermal-StressTransient Coupled Thermal-Stress
Amplitude Variation for Loading	Defines the default amplitude variation for loading magnitudes during the step.RAMP-Ramp LinearlyVaries the load magnitude linearly over the step, from the value at the end of the previous step (or from 0 at the start of the analysis) to the value specified on the loading option.STEP-InstantaneouslyApplies the load instantaneously at the beginning of the step and holds the load constant throughout the step.This option corresponds to the AMPLITUDE parameter for the *STEP keyword.	GeneralViscoImplicit DynamicThermal TransientSteady-State Coupled Thermal-StressTransient Coupled Thermal-Stress
Convert SDI	Determines how severe discontinuities, such as contact changes, are accounted for during a nonlinear analysis.Default-Previous StepUses the value specified in the previous general analysis step.YesUses local convergence criteria to determine whether a new iteration is needed. Abaqus determines the maximum penetration and estimated force errors associated with severe discontinuities and check whether these errors are within the tolerances. Therefore, a solution may converge if the severe discontinuities are small.NoForces a new iteration to occur if severe discontinuities occur during an iteration, regardless of the magnitude of the penetration and force errors.This option corresponds to the CONVERT SDI parameter for the *STEP keyword.	GeneralViscoImplicit DynamicThermal TransientSteady-State Coupled Thermal-StressTransient Coupled Thermal-Stress
Specify Matrix Storage	Controls the type of matrix storage and solution scheme to use.Default-Previous StepUses the value specified in the previous general analysis step.Symmetric MatrixUses symmetric storage and solution. Unsymmetric MatrixUses unsymmetric matrix and solution.This option corresponds to the UNSYMM parameter for the *STEP keyword.	GeneralResponse SpectrumComplex Eigenvalue ExtractionViscoImplicit DynamicDirect CyclicTransient Modal DynamicStatic PerturbationThermal TransientSteady-State Coupled Thermal-StressTransient Coupled Thermal-Stress
Extrapolation	Controls the type of extrapolation to use in a nonlinear analysis.NoSuppresses any extrapolation.ParabolicIndicates that Abaqus should use a quadratic extrapolation, in time, of the previous two incremental solutions to begin the nonlinear equation solution for the current increment.LinearIndicates that the process is essentially monotonic and that Abaqus should use a 100% linear extrapolation, in time, of the previous incremental solution to begin the nonlinear equation solution for the current increment.This option corresponds to the EXTRAPOLATION parameter for the *STEP keyword.	GeneralImplicit DynamicViscoDirect CyclicThermal TransientSteady-State Coupled Thermal-StressTransient Coupled Thermal-Stress
Linear Equation Solver	Controls whether Abaqus uses the direct sparse solver or the iterative solver for the analysis.DirectSpecifies the direct sparse matrix solver. The Abaqus direct sparse solver uses a multifront technique that can reduce the computational time required to solve the equations if the equation system has a sparse structure. This type of sparse matrix structure often occurs when the physical model is made from several connected parts, such as a spoked wheel. Parts modeled with beams, trusses, and shell elements also have sparse matrix stiffness.IterativeSpecifies the iterative linear equation solver. The Abaqus iterative solver is based on the domain decomposition method. You can only use the iterative solver for linear and nonlinear static, quasi-static, and steady-state heat transfer solution analyses. Additionally, the stiffness matrix must be symmetric and the solution must contain a single load case. The iterative solver finds an approximate solution to the linear system of equations. You should only select the Iterative option for very large, well-conditioned models (typically several million degrees of freedom). In general, the iterative solver is most appropriate for large, block-like or chunky parts. The iterative solver requires less disk storage than the direct sparse solver, but it also uses more in-core memory than the direct solver.This option corresponds to the SOLVER=ITERATIVE parameter for the Abaqus *STEP keyword.For more information, see Direct linear equation solver and Iterative linear equation solver in the Abaqus Analysis User’s Guide.	Static Perturbation
Perform Adiabatic Stress Analysis	Specifies whether to perform adiabatic stress analysis.	General
Properties (Buckling Perturbation step only)
Eigenvalue Extraction Method	Specifies the eigensolver to use for the analysis.SubspaceSpecifies the subspace iteration eigensolver.LanczosSpecifies the Lanczos eigensolver.This option corresponds to the EIGENSOLVER parameter for the *BUCKLE keyword.	Buckling Perturbation
Eigenvalue Specification	For a buckling analysis, controls the Lanczos and Subspace iteration eigenvalue extraction methods. If you set Eigenvalue Extraction Method to Subspace, lets you select either:Modes OnlySpecify the desired number of eigenvalues. Modes/Eigenvalue RangeSpecify the maximum eigenvalue of interest. The software extracts eigenvalues until either the requested number of eigenvalues has been extracted or the last eigenvalue extracted exceeds the maximum eigenvalue of interest. If you set Eigenvalue Extraction Method to Lanczos, lets you select either:Modes OnlySpecify desired number of eigenvalues. Modes/Eigenvalue RangeSpecify the minimum and/or maximum eigenvalues of interest. The software extracts the eigenvalues until either the requested number of eigenvalues has been extracted in the given range or all the eigenvalues in the given range have been extracted.	Buckling Perturbation
Estimated Number of Eigenvalues	Lets you specify the number of eigenvalues you want the software to estimate. If you want Abaqus to evaluate all the eigenvalues in the given range, specify the maximum number of expected eigenmodes.This option corresponds to the first data line for a buckling analysis.	Buckling Perturbation
Properties (Frequency Perturbation step only)
Eigenvalue Extraction Method	Specifies the eigensolver to use for the analysis.SubspaceSpecifies the subspace iteration eigensolver.LanczosSpecifies the Lanczos eigensolver.Automatic Multi-Level SubstructuringSpecifies the automatic multi-level substructuring (AMS) eigenvalue extraction method. Specify the maximum frequency of interest (the global frequency), and the software extracts all the modes up to this frequency. Note: Force or reaction nodal output variables are not valid for the AMS eigenvalue method. If you request them, the software issues an error message. This option corresponds to the EIGENSOLVER parameter for the *FREQUENCY keyword.	Frequency Perturbation
Normalization Method	Controls the normalization of eigenvectors.DisplacementAppears when Eigenvalue Extraction Method is set to Subspace or Lanczos.Normalizes the eigenvectors so the largest displacement or rotation entry in each vector is unity.MassNormalizes the eigenvectors with respect to the structure’s mass matrix. With this option, the software scales the eigenvectors so that the generalized mass for each vector is unity.This option corresponds to the NORMALIZATION parameter for the *FREQUENCY keyword.	Frequency Perturbation
Mode Generation	Appears when Eigenvalue Extraction Method is set to Subspace or Lanczos.Lets you specify whether you want the software to calculate only modes or modes and frequencies.	Frequency Perturbation
Number of Desired Modes	Appears when Eigenvalue Extraction Method is set to Subspace or Lanczos.Lets you specify the number of modes you want the software to calculate.	Frequency Perturbation
Frequency Range - Lower Limit/Frequency Range - Upper Limit	Specifies the minimum and maximum frequencies of interest in cycles/time.This option corresponds to the data lines for natural frequency extraction when EIGENSOLVER=LANCZOS, SUBSPACE, or AMS.	Frequency Perturbation
Shift Point	Appears when Eigenvalue Extraction Method is set to Subspace or Lanczos.Specifies the shifted squared frequency. Note: Specify a value when a particular frequency is of concern or when the natural frequencies of an unrestrained structure or a structure that uses secondary base motions (large mass approach) are needed.	Frequency Perturbation
Number of Vectors Used in the Iteration	Appears when Eigenvalue Extraction Method is set to Subspace.Specifies the number of vectors used in the iteration. If you omit the value, the software determines an appropriate value. In general, the convergence is faster with more vectors, but the memory requirement is larger.	Frequency Perturbation
Maximum Number of Iterations	Appears when Eigenvalue Extraction Method is set to Subspace.Specify the maximum number of iterations.	Frequency Perturbation
Block Size	Appears when Eigenvalue Extraction Method is set to Lanczos.Specifies a block size. In general, set the block size as large as the largest multiplicity of eigenvalues (that is, the largest number of modes with the same frequency). A block size of 7 is good for rigid body modes. A block size over 10 is not recommended. If you do not enter a block size, the software determines an appropriate value.	Frequency Perturbation
Maximum Number of Block Lanczos Steps	Appears when Eigenvalue Extraction Method is set to Lanczos.Specifies the maximum number of block Lanczos steps within each Lanczos run. The software usually determines the value. In general, if a particular type of eigenproblem converges slowly, providing more block Lanczos steps helps reduce the analysis cost.If you do not enter the maximum number of block steps, the software determines an appropriate value.	Frequency Perturbation
Number of Modes to Be Stored	Appears when Eigenvalue Extraction Method is set to Automatic Multi-Level Substructuring.Specifies the number of eigenvalues to be calculated. If you do not enter a value, the software evaluates all the eigenvalues from the minimum frequency of interest up to the maximum frequency of interest.	Frequency Perturbation
Cutoff Frequency Multiplier for Substructure Eigenproblems	Appears when Eigenvalue Extraction Method is set to Automatic Multi-Level Substructuring.Specifies the cutoff frequency for substructure eigenproblems, defined as a multiplier of the maximum frequency of interest. Note: You control the execution of the AMS method using the three cutoff parameters. These three parameters multiplied by the maximum frequency of interest define three cutoff frequencies. The Cutoff Frequency Multiplier for Substructure Eigenproblems parameter controls the cutoff frequency for substructure eigenproblems in the reduction phase, while the First Cutoff Frequency Multiplier Used to Define a Starting Subspace and Second Cutoff Frequency Multiplier Used to Define a Starting Subspace parameters control the cutoff frequencies used to define a starting subspace in the reduced eigensolution phase. In general, increasing the value of First Cutoff Frequency Multiplier Used to Define a Starting Subspace and Second Cutoff Frequency Multiplier Used to Define a Starting Subspace improves the accuracy of the results but can affect the performance of the analysis.	Frequency Perturbation
First Cutoff Frequency Multiplier Used to Define a Starting Subspace	Appears when Eigenvalue Extraction Method is set to Automatic Multi-Level Substructuring.Specifies the first cutoff frequency used to define a starting subspace in the reduced eigensolution phase, defined as a multiplier of the maximum frequency of interest. The first cutoff frequency must be a value greater than the cutoff frequency multiplier value for Cutoff Frequency Multiplier Used to Define a Starting Subspace.	Frequency Perturbation
Second Cutoff Frequency Multiplier Used to Define a Starting Subspace	Appears when Eigenvalue Extraction Method is set to Automatic Multi-Level Substructuring.Specifies the second cutoff frequency used to define a starting subspace in the reduced eigensolution phase, defined as a multiplier of the maximum frequency of interest. The second cutoff value must be greater than 1.0 and less than the cutoff frequency multiplier value for Cutoff Frequency Multiplier for Substructure Eigenproblems.	Frequency Perturbation
Activate SIM Software Architecture	Appears when Eigenvalue Extraction Method is set to Subspace or Lanczos.Controls whether the subsequent mode-based linear dynamic analysis steps should use the high-performance versions based on the Abaqus SIM software architecture. Note: The SIM architecture is available in Abaqus version 6.13 and higher.This option corresponds to the SIM parameter for the *FREQUENCY keyword.For more information, see TSIM architecture in the Abaqus environment and Using the SIM architecture for modal superposition dynamic analyses in the Abaqus Analysis User’s Guide.	Frequency Perturbation
Project Viscous and Structural Damping Coefficients	Appears when the Activate SIM Software Architecture check box is selected and Eigenvalue Extraction Method is set to Lanczos.Controls the projection of the viscous and structural damping operators during the natural frequency extraction procedure.Select the Project Viscous and Structural Damping Coefficients check box to project the viscous and structural damping operators during the natural frequency extraction procedure. If there is no damping defined in the model, the projection is not performed.Clear the Project Viscous and Structural Damping Coefficients check box if you do not want to project the damping operators.This option corresponds to the DAMPING PROJECTION parameter for the *FREQUENCY keyword.	Frequency Perturbation
Compute Residual Modes	Appears when Eigenvalue Extraction Method is set to Lanczos or Automatic Multi-Level Substructuring.Select this check box to indicate that residual modes are to be computed. The residual modes help correct for errors introduced by mode truncation.Note: To minimize the number of modes required for a sufficient degree of accuracy, the set of eigenmodes used in the projection and superposition can be augmented with additional modes known as residual modes. If you select the Compute Residual Modes check box to compute residual modes, do not enter a value for Number of Desired Modes.	Frequency Perturbation
Request Eigenvectors at Specified Nodes	Appears when Eigenvalue Extraction Method is set to Automatic Multi-Level Substructuring.Specifies how to request eigenvectors.All NodesComputes eigenvectors at all nodes.Automatically Selected by SolverLets the software automatically selects the nodes at which to compute eigenvectors.Select Node SetSpecifies a node set. The software computes and stores eigenvectors at the nodes that belong to that node set.	Frequency Perturbation
Specify a Node Set	Appears when Eigenvalue Extraction Method is set to Automatic Multi-Level Substructuring and Request Eigenvectors at Specified Nodes is set to Select Node Set.Specifies a node set. Select the node set from the list or click New Group to create a node set. Note: When you create a group of nodes, be sure to enter the labels in the Node Labels group, the only entity type supported.The node set that you specify must include all nodes at which loads are applied or output is requested in any subsequent modal analysis. If element output is requested or element-based loading is applied, the nodes attached to the associated elements must also be included in this node set. Computing eigenvectors at only selected nodes improves performance and reduces the amount of stored data.If a mismatch exists between the group of nodes at which eigenvectors will be computed and the group of element/nodal output requested in output requests, the solver issues an error message.	Frequency Perturbation
Directional and Modal Summation Methods
Peak Response Combination	Specifies how to combine the individual excitations.Unidirectional ExcitationSet to ignore the COMP option.SSRSSet to use the square root of the sum of the squares. If this parameter is used, the modal summation is performed first, followed by the summation of the directional excitation components.AlgebraicSet to the sum the directional excitation components algebraically. If this parameter is used, the directional excitation components are summed first, followed by the modal summation.R40Set to use the 40% rule as recommended by the ASCE 4–98 Guide that assumes that for the maximum response from one component, the responses from the other two components are 40% of their maximum value.R30Set to use the 30% rule. This rule assumes that for the maximum response from one component, the responses from the other two components are 30% of their maximum value. It follows the expressions for the 40% rule as described in the ASCE 4–98 Guide.This option corresponds to the COMP parameter in the *RESPONSE SPECTRUM keyword.	Response Spectrum
Summation Method	Controls the summation method used. Absolute ValueSet to sum the absolute values of the responses in each natural mode.Complete Quadratic ComputationSet to use the complete quadratic combination method to sum the responses in each natural mode.Double Sum CombinationSet to use the double sum combination method, which is the first attempt to evaluate modal correlation based on random vibration theory. It uses the time duration tD of strong earthquake motion. Grouping MethodSet to use the grouping method as described in USNRC Regulatory Guide 1.92, February 1976.Naval Research Laboratory MethodSet to use the Naval Research Laboratory method. Square Root of the Sum of Squares SummationSet to use the square root of the sum of squares summation.Ten Percent MethodSet to use the Ten Percent Method.This option corresponds to the SUM parameter in the *RESPONSE SPECTRUM keyword.	Response Spectrum
Temperature Pre-Load
Pre-Load Type	If you want to specify temperature as a pre-defined Abaqus field for the analysis, use this option to read in the temperature data from a results file generated during a previous analysis. Select the type of results file from the list and then select the file.This option corresponds to the *TEMPERATURE keyword.	GeneralImplicit DynamicViscoDirect CyclicDynamic ExplicitSteady-State Coupled Thermal-StressTransient Coupled Thermal-StressDynamic Coupled Thermal-Stress
Force Pre-Load
Pre-Load Type	If you want to apply force data from a previous analysis, use this option to read in the results file that contains the data.This option corresponds to the *CLOAD keyword.	GeneralImplicit DynamicViscoDynamic ExplicitSteady-State Coupled Thermal-StressTransient Coupled Thermal-StressDynamic Coupled Thermal-Stress
Response Spectrum First (Response Spectrum step only)**Response Spectrum Second (Optional)**Response Spectrum Third Direction (Optional)
Second and third direction data is only required when the individual peak responses to the excitations in different directions occurs at different times, and, therefore, must be combined into an overall peak response. The directions defined by the direction cosines of the independent responses must be orthogonal.
Select Spectrum	Specifies a Spectrum modeling object. This option corresponds to the *SPECTRUM keyword.Select an existing modeling object from the list or click Create Modeling Object to create a new one.Click Edit to edit the selected modeling object.For more information, see Spectrum dialog box (Abaqus).	Response Spectrum
X-direction Cosine	Sets the X-direction cosine of this direction.	Response Spectrum
Y-direction Cosine	Sets the Y-direction cosine of this direction.	Response Spectrum
Z-direction Cosine	Sets the Z-direction cosine of this direction.	Response Spectrum
Multiplying Factor	Sets the factor multiplying the magnitudes in the response spectrum. The default is 1.0.	Response Spectrum
Substructure Data
Substructure Identifier, Z:	Specifies a unique identifier to be assigned to the substructure in the substructure library. The identifier must begin with the letter Z followed by a number no larger than 9999. If a substructure with the same identifier already exists in the library, the solve terminates with an error message unless you specified that the existing substructure should be overwritten using the Overwrite Existing Substructure check box.	Substructure Generation
Overwrite Existing Substructure	Overwrites the existing substructure.	Substructure Generation
Model Data	Specifies whether or not to generate the model data file (.odb).ODBForces the generation of the model data file.NoneSuppresses the generation of the model data file.	Substructure Generation
Generate Matrix TypeFor information about how the matrices are generated, see Generating global matrices in the Abaqus Analysis User's Guide.
Stiffness Matrix	Generates a stiffness matrix.	Matrix Generation
Mass Matrix	For a matrix generation step, generates a mass matrix. For a substructure generation step, generates a reduced mass matrix.	Matrix GenerationSubstructure Generation
Viscous Damping Matrix	For a matrix generation step, generates a viscous damping matrix. For a substructure generation step, generates a reduced viscous damping matrix.	Matrix GenerationSubstructure Generation
Structural Damping Matrix	For a matrix generation step, generates a structural damping matrix. For a substructure generation step, generates a reduced structural damping matrix.	Matrix GenerationSubstructure Generation
Load Matrix	Generates a load matrix.	Matrix Generation
Generation Procedure
Matrix Generation Procedure	Specifies that the software generate global or local element matrices. Global Assembled MatricesGenerates global matrices for a model in assembled form. The generated global matrices are assembled from the local element matrices and include contributions from matrix input data. Local Element MatricesGenerates local element matrices.	Matrix Generation
Model Subset
Matrix Generation Element Selection	Specifies that the software generate matrices for the entire model or specified elements Entire ModelGenerates matrices for the entire model.Specified ElementsGenerates matrices for a portion of the model that an element set defines.	Matrix Generation
Matrix Generation Element Set	Appears when Matrix Generation Element Selection is set to Specified Elements. Select a group from the list as the element set to be used for matrix generation or use the New Group tool to create a new group.	Matrix Generation
Source Contribution	Specifies the type of source from which to generate the matrices. AllGenerates matrices using contributions from both the finite elements and the matrix input data used in the FE model.Finite ElementsGenerates matrices using contributions from only the finite elements.Matrix InputGenerates matrices using contributions from only the matrix input data.	Matrix Generation
Physical Field	Lets you define the portion of the model to be used for matrix generation based on the physical field (structural and acoustic).AllGenerates the matrices using both the structural and acoustic portions of the model.StructuralGenerates the matrices using only the structural portion of the model.AcousticGenerates the matrices using only the acoustic portion of the model. Note: Acoustic elements are not supported in the Abaqus environment. If you select to generate matrices based on acoustic elements, an error message appears.	Matrix Generation
Recovery Matrix
Enable Recovery	Specifies whether or not the recovery of element or nodal information is required within the substructure. Clearing the Enable Recovery check box significantly reduces the size of the substructure database for a large substructure because it does not store the information needed to recover eliminated variables.	Substructure Generation
Selective Recovery Method	Lets you select recovery for the entire model or a subset of the internal degrees of freedom. Selecting only a subset (elements or nodes) reduces disk usage substantially.Entire ModelDefines the entire model as the recovery set.Specified ElementsDefines an element set for selective recovery. Specified NodesDefines a node set for selective recovery.	Substructure Generation
Recovery Matrix Element/ Recovery Matrix Node Set	Specifies the frequency at which to evaluate frequency-dependent material properties specified in the model definition (viscoelasticity, springs, and dashpots) for use in generating the matrix.If you do not specify a value, the solver evaluates the stiffness associated with frequency-dependent springs and dashpots at zero frequency and does not consider the stiffness contributions from frequency-domain viscoelasticity.	Matrix GenerationSubstructure Generation
Apply Multipoint Constraints
Generate Matrices with Applied Multipoint Constraints	If multipoint constraints are used in the model, generates the matrices with the applied multipoint constraints. The generated matrices include entries only for the independent degrees of freedom.Clear the selection of the Generate Matrices with Applied Multipoint Constraints check box to not apply the multipoint constraints in the generated model.
Friction Damping
Ignore Friction-induced Viscous Damping Effects	Lets you not include friction-induced viscous damping effects.	Matrix GenerationSubstructure Generation
Nodes to be Visible in the Matrix Usage Model
Public Nodes	Specifies which nodes are visible in the matrix usage model. All User-defined NodesSpecifies that all user-defined nodes are visible in the matrix usage model. Specified NodesSpecifies the node set that contains all the nodes that are presented as user-defined nodes during matrix input; all other nodes are designated as internal nodes and effectively hidden.	Matrix Generation
Public Nodes	Appears when Public Nodes is set to Specified NodesSpecify a group of nodes or use the New Group tool create a new group.	Matrix Generation
Gravity Load
Calculate Substructure Gravity Load Vectors	Calculates the substructure's gravity load vectors during substructure generation to define gravity loading that acts in a fixed global direction during usage. In this case, gravity loading should not be defined as part of a substructure load case. When Abaqus calculates the gravity load vectors, it generates a gravity load vector for each global direction.	Substructure Generation
Substructure Eigenvalue Problem
Enable Solving Substructure Eigenvalue Problem	If a generated substructure has the reduced mass matrix, enables solving of the substructure eigenvalue problem.For more information about how Abaqus solves the substructure eigenvalue problem, see Using substructures in the Abaqus Analysis Guide.	Substructure Generation
Boundary Condition Control Variables
Evaluation Time/Evaluation Temperature	Specifies the value used to evaluate a time- or temperature-dependent boundary condition when you use the boundary condition in a solution that does not support dependent boundary conditions. Select the type of results file from the list and then select the file.The software first uses the field evaluation value for the step to determine the loading value. If no field evaluation value is defined for the step, the software uses the field evaluation value for the solution.	All step types

Look up more details

Solution Step dialog box tabs (Abaqus)

Solution Step dialog box (Abaqus), Change Friction page

Solution Step dialog box (Abaqus), Complex Eigenvalue Extraction

Solution Step dialog box (Abaqus), Control Parameters page

Solution Step dialog box (Abaqus), Dynamic Coupled Heat Transfer and Stress Setup Step page

Solution Step dialog box (Abaqus), Cyclic Symmetry Modes page

Solution Step dialog box (Abaqus), Cyclic Step Setup page

Solution Step dialog box (Abaqus), Data Line page

Solution Step dialog box (Abaqus), Coupled Heat Transfer and Stress Setup Step page

Solution Step dialog box (Abaqus), Explicit Dynamic Step Setup page

Solution Step dialog box (Abaqus), Heat Transfer Setup page

Solution Step dialog box (Abaqus), Implicit Dynamic Step Setup page

Solution Step dialog box (Abaqus), Mass Scaling page

Solution Step dialog box (Abaqus), Other Step Options page

Solution Step dialog box (Abaqus), Other Step Parameters page

Solution Step dialog box (Abaqus), Output page

Solution Step dialog box (Abaqus), Steady-State Modal Dynamic Step Parameters page

Solution Step dialog box (Abaqus), Transient Modal Dynamic Step Setup page

Solution Step dialog box (Abaqus), User Defined Text page

Solution Step dialog box (Abaqus), Visco Step Setup page

Solution Step dialog box (Abaqus), General page, 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 } });