Solution dialog box (ANSYS)

Option	Description	Supported solutions	ANSYS Command
Preview Solution Setup	Generates a preview of the ANSYS input file with your current selections. For more information, see Previewing ANSYS solver syntax.
Description	Opens an editor that lets you enter a description for the solution.	All solutions	-
Scratch Directory	For all analysis types, you can specify a path where the results will be stored.	All solutions	/ASSIGNBasic Analysis Guide: File Management and Files
Run Job in Foreground	Solves the solution in the foreground and freezes Pre/Post so that you cannot make changes to your model during the solve.Clear this check box to be able to access this software while solving the solution.	All solutions	-Operations Guide: Batch Mode

General page

Option	Description	Supported solution types	ANSYS Command
Inertia Relief	Controls whether the solver performs inertial relief calculations.	Linear StaticsModal	IRLFSee the ANSYS Commands Reference.
Algorithm (EQSLV)	Specifies the type of equation solver to use for the solution:Choose Sparse to use the sparse direct equation solver.Choose PCG to use the Pre-conditioned Conjugate Gradient iterative solver.Choose JCG to use the Jacobi Conjugate Gradient iterative equation solver.	Linear StaticsModalLinear BucklingNonlinear StaticsHarmonic - Full MethodHarmonic - Mode SuperpositionTransient Dynamic - Full MethodTransient Dynamic - Mode SuperpositionCoupled-Fields Thermal-StructuralSteady State ThermalTransient Thermal	EQSLV, SPARSEEQSLV, PCGEQSLV, JCGSee the ANSYS Basic Analysis Guide: Solution, Selecting a Solver
Difficulty Level (PCGOPT, Lev_diff)	Available when Algorithm (EQSLV) is set to PCG or when Algorithm (MODOPT) is set to (LANPCG) PCG Lanczos.Indicates the level of difficulty of the analysis. Lower values (1 or 2) generally provide the best results for problems that are well conditioned. Higher values typically require more memory.	Linear StaticsModalLinear BucklingNonlinear StaticsHarmonic - Full MethodHarmonic - Mode SuperpositionTransient Dynamic - Full MethodTransient Dynamic - Mode SuperpositionCoupled-Fields Thermal-StructuralSteady State ThermalTransient Thermal	PCGOPT, Lev_diff
Reduce I/O (PCGOPT_ReduceIO)	Available when Algorithm (EQSLV) is set to PCG or when Algorithm (MODOPT) is set to (LANPCG) PCG Lanczos.Controls whether the software attempts to reduce the I/O performed during the equation solution to reduce the overall solve time.	Linear StaticsModalLinear BucklingNonlinear StaticsHarmonic - Full MethodHarmonic - Mode SuperpositionTransient Dynamic - Full MethodTransient Dynamic - Mode SuperpositionCoupled-Fields Thermal-StructuralSteady State ThermalTransient Thermal	PCGOPT_ReduceIO
Sturm Sequence Check (PCGOPT,StrmCk)	Available when Algorithm (EQSLV) is set to PCG or when Algorithm (MODOPT) is set to (LANPCG) PCG LanczosControls whether the software performs a Sturm sequence check during the analysis. If you select this option, the software performs a factorization that requires significant memory for the extra computations.	Linear StaticsModalLinear BucklingNonlinear StaticsHarmonic - Full MethodHarmonic - Mode SuperpositionTransient Dynamic - Full MethodTransient Dynamic - Mode SuperpositionCoupled-Fields Thermal-StructuralSteady State ThermalTransient Thermal
Write .FULL file (PCGOPT,Wrtfull)	Available when Algorithm (EQSLV) is set to PCG or when Algorithm (MODOPT) is set to (LANPCG) PCG Lanczos.Controls whether ANSYS writes out the .FULL file.	Linear StaticsModalLinear BucklingNonlinear StaticsHarmonic - Full MethodHarmonic - Mode SuperpositionTransient Dynamic - Full MethodTransient Dynamic - Mode SuperpositionCoupled-Fields Thermal-StructuralSteady State ThermalTransient Thermal
Memory mode when Lev_Diff#5 (PCGOPT,Memory)	Available when Algorithm (EQSLV) is set to PCG or when Algorithm (MODOPT) is set to (LANPCG) PCG Lanczos.When Difficulty Level (PCGOPT, Lev_diff) is set to 5, controls whether ANSYS performs the solve in-core or out of core.	Linear StaticsModalLinear BucklingNonlinear StaticsHarmonic - Full MethodHarmonic - Mode SuperpositionTransient Dynamic - Full MethodTransient Dynamic - Mode SuperpositionCoupled-Fields Thermal-StructuralSteady State ThermalTransient Thermal
MPC184 Lagrange Multiplier (PCGOPT,LM_Key)	Available when Algorithm (EQSLV) is set to PCG or when Algorithm (MODOPT) is set to (LANPCG) PCG Lanczos.Controls whether the software uses the Lagrange multiplier method for all MPC184 elements.	Linear StaticsModalLinear BucklingNonlinear StaticsHarmonic - Full MethodHarmonic - Mode SuperpositionTransient Dynamic - Full MethodTransient Dynamic - Mode SuperpositionCoupled-Fields Thermal-StructuralSteady State ThermalTransient Thermal
Memory Allocation Option (BCSOption,Memory_Option)	Available when Algorithm (EQSLV) is set to Sparse.Controls how the solver uses memory during the solution.	Linear StaticsModal
Initial Memory Allocation Option (BCSOption, Memory_Size)	Available when Algorithm (EQSLV) is set to Sparse.	Linear StaticsModal
Additional Output Printing (BCSOPTION,Solve_Info)	Available when Algorithm (EQSLV) is set to Sparse.Lets you specify the initial memory size allocation for the sparse solver in MB.	Linear StaticsModal
Large Displacements	Controls whether the software includes large-deflection effects in a static or full transient analysis.Select the Large Displacements check box to include large-deflection effects.Clear the Large Displacements check box to ignore large deflection effects.	Nonlinear Statics	NLGEOMSee the ANSYS Structural Analysis Guide: Nonlinear Structural Analysis
Mode Generation	Controls whether you specify the number of modes to extract or the frequency range of interest.	Modal	Mode/Frequency: MODOPT,,,FREQB, FREQEMode Only: MODOPT,,,FREQBSee the Structural Analysis Guide: Modal Analysis
Number of Modes	Lets you specify the number of modes to extract.	Modal	MODOPT,,NMODESee the ANSYS Structural Analysis Guide: Modal Analysis
Frequency Range	Lets you specify the beginning (lower end) and ending (upper end) of the frequency range of interest.	Modal	MODOPT,,FREQB, FREQESee the ANSYS Structural Analysis Guide: Modal Analysis
Solution Tolerance (EQSLV, TOLER)	When you select either JCG or PCG from the Algorithm list, specifies the iterative solver tolerance value.	Linear StaticsModalBucklingHarmonic - Full MethodHarmonic - Mode SuperpositionThermal	EQSLV,, TOLER,See the ANSYS Commands Reference
Solution Multiplier	When you select PCG from the Algorithm list, controls the maximum number of iterations the software performs during convergence calculations. The maximum number of iterations is equal to the specified Solution Multiplier value times the number of degrees of freedom (DOF). The solver continues to iterate until it reaches the maximum number of iterations or the solution converges.	Linear StaticsModalBucklingThermal	EQSLV,, MULTSee the ANSYS Commands Reference
Default Temperature (TREF)	Specifies a uniform starting temperature, which is the temperature that is in effect at the beginning of the analysis.	Linear StaticsBucklingNonlinear StaticsHarmonic - Full MethodHarmonic - Mode SuperpositionThermalCoupled-Fields Thermal-StructuralModal Flexible Body	TREFSee the ANSYS Commands Reference
Lumped Mass Matrix Formulation (LUMPM)	Uses the lumped mass approximation formulation instead of the element-dependent default mass matrix formulation.	Modal Flexible Body	LUMPMSee the ANSYS Commands Reference.
Material plasticity model (stress-strain)	Lets you specify the plasticity model to use.	Nonlinear StaticsTransient Dynamic - Full MethodTransient Dynamic - Mode SuperpositionCoupled-Fields Thermal-Structural	TB,MELASTB,MISOTB,KIHNSee the ANSYS Commands Reference
Time at the end of Step (TIME)	Lets you specify the ending time for a load step.	Linear StaticsModalBucklingNonlinear StaticsThermal	TIMESee the ANSYS Commands Reference
Use radiation to apply flame temperature on SURF152 extra node	Lets you define the radiation effect of a flame on a surface, given the temperature of the flame and the emissivity of the surface.For more information, see Applying a flame temperature to SURF152 elements.	Thermal
Loading Variation (KBC)	Specifies stepped or ramped loading within the solution.	Harmonic - Full MethodHarmonic - Mode Superposition	KBCSee the ANSYS Commands Reference
Algorithm (MODOPT)	Specifies the mode extraction method to use for the analysis.Select Lanczos to use the Block Lanczos eigenvalue extraction method.Select Subspace to use the subspace iteration method.Select Householder to use the reduced method.Select Unsymmetric to use the unsymmetric eigensolver.Select Damped system to use the damped eigensolver.Select Damped QR to use the QR damped method for determining the complex eigenvalues and corresponding eigenvectors of damped linear systems.Select Variational to solver with the Variational Technology method.	Modal	MODOPT, LANB, SUBSP, REDUC, UNSYM, DAMP, QRDAMP, or VTSee MODOPT in the ANSYS Commands Reference or Eigenvalue and Eigenvector Extraction in the ANSYS Theory Reference manual.
Normalize Mode Shapes to (MODOPT,,,,,,NmKey)	Controls how the software normalizes the mode shapes. Select (OFF) The mass matrix to normalize the mode shapes to the mass matrix. Select this option if you plan to perform a subsequent spectrum or mode-superposition analysis.Note: This option is invalid for damped modal cyclic symmetry (If Algorithm (MODOPT) is set to (DAMP) Damped or (QRDAMP) Damped QR in a Modal solution with cyclic symmetry).Select (ON) To unity to normalize the mode shapes to unity. In ANSYS, this option is the default setting for modal cyclic symmetry analyses.	ModalModal Flexible BodyHarmonic - Full MethodTransient Dynamic - Mode Superposition	Nrmkey for the MODOPT command.See the ANSYS Commands Reference
NSUBST
Number of Substeps (NSBSTP)	Specifies the number of substeps for this load step.	Nonlinear Statics	NSBSTPSee the ANSYS Basic Analysis Guide: Loading
**Minimum Number of Substeps (NSBMN)**Maximum Number of Substeps (NSBMX)	Specifies the minimum and maximum number of substeps for this load step.	Nonlinear Statics	NSBMX, NSBMNSee the ANSYS Basic Analysis Guide: Loading
Automatic Master Degrees of Freedom Generation (TOTAL)
Total Number of Master DOF	Available when Algorithm is set to Householder.Lets you specify the total number of master degrees of freedom to use in the analysis.	Modal	TOTAL: NTOTSee the ANSYS Commands Reference
Rotational Masters Key	Controls whether the software includes all degrees of freedom, including rotational degrees of freedom, in the automatic master DOF selection.	Modal	TOTAL: NRMDFSee the ANSYS Commands Reference
Master Degrees of Freedom Generation (M)
Node Group to Use	Available when Algorithm is set to Householder.Selects the group that contains the master DOF.Select an existing group from the list, or click New Group to create, manage, or select groups.See Groups for more information.	Modal	M: NODESee the ANSYS Commands Reference
Translational DOF	Specifies the translational DOF to which the master degrees of freedom apply.	Modal	M: Lab1See the ANSYS Commands Reference
Rotational DOF	Specifies the rotational DOF to which the master degrees of freedom apply.	Modal	M: Lab1See the ANSYS Commands Reference

Harmonic Options

Option	Description	Supported solutions	ANSYS Command
Forcing Frequency Range in Harmonic (HARFREQ)
**Start Frequency (FREQB)**End Frequency (FREQE)	Specifies the beginning and ending frequency points for the solution.	Harmonic - Full MethodHarmonic - Mode Superposition	FREQB and FREQESee the ANSYS Commands Reference
Logarithm Frequency Span (LogOpt)	Defines the frequency span of the logarithm.	Harmonic - Full MethodHarmonic - Mode Superposition	See the ANSYS Commands Reference
Forcing Frequency Table (FREQARR)	Lets you specify the appropriate Forcing Frequency Table modeling object that lists the forcing frequencies.	Harmonic - Full MethodHarmonic - Mode Superposition	See the ANSYS Commands Reference
Frequency Table versus Range Tolerance (Toler)	Specifies the tolerance value that ANSYS applies to the frequency table.	Harmonic - Full MethodHarmonic - Mode Superposition	See the ANSYS Commands Reference
Number of Harmonic Solutions (NSUBST)
Number of Solutions (NBSTP)	Controls how many harmonic solutions that ANSYS calculates. ANSYS evenly spaces these solutions within the specified frequency range.	Harmonic - Full MethodHarmonic - Mode Superposition	NSUBST, NBSTPSee the ANSYS Commands Reference
**Minimum Number of Solutions (NSBMN)**Maximum Number of Solutions (NSBMX)	Lets you specify the maximum and minimum number of harmonic solutions to calculate.	Harmonic - Full MethodHarmonic - Mode Superposition	NSUBST, NSBMN or NSBMXSee the ANSYS Commands Reference
Lumped Mass Matrix Formulation (LUMPM)	Controls whether ANSYS uses the element-dependent default mass matrix formulation or the lumped mass approximation formulation.	Harmonic - Full MethodHarmonic - Mode Superposition	LUMPMSee the ANSYS Commands Reference

Damping

Option	Description	Supported solutions	ANSYS Command
Mass Damping Coefficient (ALPHAD)	Specifies the mass damping coefficient.	Harmonic - Full MethodHarmonic - Mode Superposition	ALPHADSee the ANSYS Commands Reference
Stiffness Damping Coefficient (BETAD)	Specifies the stiffness damping coefficient.	Harmonic - Full MethodHarmonic - Mode Superposition	BETADSee the ANSYS Commands Reference
Constant Structural Damping Coefficient (DMPSTR)	Defines the coefficient for constant structural damping.	Harmonic - Full MethodHarmonic - Mode Superposition	DMPSTRSee the ANSYS Commands Reference

Generation Pass page

Option	Description	Supported solution types	ANSYS Command
Component Mode Synthesis Options (CMSOPT)
Method (CMSMETH)	Specifies the component mode synthesis (CMS) method to use, either fixed-interface, free-interface, or residual-flexible free-interface.	Modal Flexible Body	CMSOPTSee the ANSYS Commands Reference.
Number of Modes (NMODE)	Sets the number of normal modes extracted and used for the superelement generation. The value must be a minimum of one.	Modal Flexible Body	CMSOPTSee the ANSYS Commands Reference.
Frequency Range - Lower Limit (FREQB)	Specifies the beginning, or lower end, of the frequency range of interest.	Modal Flexible Body	CMSOPTSee the ANSYS Commands Reference.
Frequency Range - Upper Limit (FREQE)	Specifies the ending, or upper end, of the frequency range of interest.	Modal Flexible Body	CMSOPTSee the ANSYS Commands Reference.
Method to Define Free Body Modes (FBDDEF)	Available when Method (CMSMETH) is set to (FREE) Free-interface or (RFFB) Residual-flexible free-interface.Specifies the method to use for defining free body modes.(FNUM) Number of rigid body modesUses the number of rigid body modes in the calculation.(FTOL) Specify toleranceUses a specified tolerance to determine the rigid body modes in the calculation.(FAUTO) Automatically determine rigid body modesAutomatically determines rigid body modes in the calculation.(RIGID) User-defined rigid body modesLets you define rigid body modes.	Modal Flexible Body	CMSOPTSee the ANSYS Commands Reference.
Number of rigid body modes (FBDVAL)	Appears when Method to Define Free Body Modes (FBDDEF) is set to (FNUM) Number of rigid body modes.Specifies the number of rigid body nodes.	Modal Flexible Body	CMSOPTSee the ANSYS Commands Reference.
Tolerance (FBDVAL)	Appears when Method to Define Free Body Modes (FBDDEF) is set to (FTOL) Specify tolerance.Specifies the tolerance to use, where the value is a positive real number representing rad/sec.	Modal Flexible Body	CMSOPTSee the ANSYS Commands Reference.
Rigid body modes, all direction (RIGID,ALL) Rigid body modes, X direction (RIGID,UX) Rigid body modes, Y direction (RIGID,UY) Rigid body modes, Z direction (RIGID,UZ) Rigid body modes, X rotation (RIGID,ROTX) Rigid body modes, Y rotation (RIGID,ROTY) Rigid body modes, Z rotation (RIGID,ROTZ)	Appears when Method to Define Free Body Modes (FBDDEF) is set to (RIGID) User-defined rigid body modes.Specifies up to six global Cartesian directions of rigid modes. For a completely free 2D model, do one of the following:Select the Rigid body modes, all direction (RIGID,ALL) check box. Clear the Rigid body modes, all direction (RIGID,ALL) check box and define the X and Y directions and the Z rotation. For a completely free 3D model, do one of the following:Select the Rigid body modes, all direction (RIGID,ALL) check box. Clear the Rigid body modes, all direction (RIGID,ALL) check box and select all of the six other directions and rotations. For a constrained model, clear the selection of the Rigid body modes, all direction (RIGID,ALL) check box and select one of the other directions or rotations, as appropriate, to specify each and every unconstrained direction that exists in the model (not specifying every direction can cause difficulties in extracting the modes). To force the subspace iteration calculation of all rigid body modes, clear all the check boxes.	Modal Flexible Body	RIGIDSee the ANSYS Commands Reference.
Output Control Key (IOKEY)	Specifies how the transformation matrix is output.(TCMS) Write transformation matrixWrites the transformation matrix of the nodal component to a .tcms file.(EXB) Write body propertyWrites a body property input file (.exb) containing the condensed substructure matrices and other body properties.	Modal Flexible Body	CMSOPTSee the ANSYS Commands Reference.
Substructure Analysis Options (SEOPT)
Output Matrix File Name (Sname.SUB)	Sets the name for the superelement matrix file. The matrix file name format is Sename.SUB, where Sename is the name you type.	Modal Flexible Body	SEOPTSee the ANSYS Commands Reference.
Matrix Generation Key (SEMATR)	Specifies what the software should generate.(1) Generate stiffness matrixGenerates a stiffness (or conductivity) matrix.(2) Generate stiffness and mass matricesGenerates a stiffness and mass (or conductivity and specific heat) matrices.(3) - Generate stiffness, mass and damping matricesGenerates stiffness, mass, and damping matrices.	Modal Flexible Body	SEOPTSee the ANSYS Commands Reference.
Print Key (SEPR)	Specifies whether to print matrices and/or load vectors.	Modal Flexible Body	SEOPTSee the ANSYS Commands Reference.
Stress Stiffening Key (SESST)	Specifies whether or not to save space for the stress stiffening calculated in a generation that is run after the expansion pass.	Modal Flexible Body	SEOPTSee the ANSYS Commands Reference.
**Expansion Pass Method (ExpMth)**FBDVAL	Specifies the method for the Expansion Pass:(BACKSUB) Save necessary factorized matrix filesSaves necessary factorized matrix files for back-substitution during subsequent expansion passes. This option usually uses a large amount of disk.(RESOLVE) Do not saveDoes not save factorized matrix files, which saves disk space. Global stiffness matrix is reformed during the Expansion Pass. You cannot use the Expansion Pass Method (ExpMth) option if the Use Pass uses large deflections.	Modal Flexible Body	SEOPTSee the ANSYS Commands Reference.

Use Pass (Modal) page

Option	Description	Supported solution types	ANSYS Command
Mode Generation	Sets the mode generation method for the modal analysis.	Modal Flexible Body
Number of Modes	Specifies the number of modes to extract. Note: When Algorithm (MODOPT) is set to (SUBSP) Subspace iteration, the number of modes should be less than half the total number of degrees of freedom.	Modal Flexible Body	MODOPTSee the ANSYS Commands Reference.
Frequency Range - Lower Limit	Appears when Mode Generation is set to Modes/FrequencySpecifies the beginning, or lower end, of the frequency range of interest.When Algorithm (MODOPT) is set to (SUBSP) Subspace iteration, (LANB) Block Lanczos, (UNSYM) Unsymmetric matrix, or (DAMP) Damped, the frequency lower limit also represents the first shift point for the eigenvalue iterations. It defaults to -1.0 if you type 0 or if you leave it blank for the subspace iteration, unsymmetric matrix, or damped extraction methods.Eigenvalue extraction is most accurate near the shift point. The subspace iteration and block Lanczos methods use the multiple shift points. For the subspace iteration method and for the unsymmetric matrix, block Lanczos, and damped methods with a positive frequency lower limit, the software outputs the eigenvalues beginning at the shift point and they increase in magnitude. For the unsymmetric matrix and damped methods with a negative frequency lower limit, the software outputs the eigenvalues beginning at zero magnitude and increase.	Modal Flexible Body	MODOPTSee the ANSYS Commands Reference.
Frequency Range - Upper Limit	Appears when Mode Generation is set to Modes/Frequency.Specifies the ending, or upper end, of the frequency range of interest. The upper limit frequency defaults to 1e8 for when Algorithm (MODOPT) is set to (SUBSP) Subspace iteration or (LANB) Block Lanczos. The default for the other methods is to calculate all modes, regardless of their maximum frequency.	Modal Flexible Body	MODOPTSee the ANSYS Commands Reference.
Algorithm (MODOPT)	Specifies the extraction method.The unsymmetric matrix and damped extraction methods cannot be followed by a spectrum analysis.	Modal Flexible Body	MODOPTSee the ANSYS Commands Reference.

Expansion Pass page

The Expansion Pass step obtains the name of the superelement matrix file from the Generation Pass step and the name of the modal results file from the Use Pass step.

Option	Description	Supported solution types	ANSYS Command
Solutions to be Expanded (NUMEXP)
Expand to	Specifies to either expand all solutions or a range of solutions from analyses that use reduced or mode superposition methods.	Modal Flexible Body	NUMEXPSee the ANSYS Commands Reference.
Number of Solutions (Num)	Appears when Expand to is set to (Num) Solution range.Specifies the number of evenly spaced solutions to expand between the frequency ranges you specify in Beginning Frequency Range (BEGRNG) and Ending Frequency Range (ENDRNG).	Modal Flexible Body	NUMEXPSee the ANSYS Commands Reference.
Beginning Frequency Range (BEGRNG)	Appears when Expand to is set to (Num) Solution range.Specifies the beginning time (or frequency) range for expanded solutions.The first expansion is done at the first point beyond the beginning range (BEGRNG. That is, at BEGRNG + (ENDRNG - BEGRNG)/NUM.	Modal Flexible Body	NUMEXPSee the ANSYS Commands Reference.
Ending Frequency Range (ENDRNG)	Appears when Expand to is set to (Num) Solution range.Specifies the ending time (or frequency) range for the expanded solutions.	Modal Flexible Body	NUMEXPSee the ANSYS Commands Reference.
Element Calculation Key (Elcalc)	Specifies whether or not to calculate element results, nodal results, and reaction loads. If you want to obtain output on elements, Element Calculation Key (Elcalc) must be set to (YES) Calculate element results, nodal loads, and reaction loads.	Modal Flexible Body	NUMEXPSee the ANSYS Commands Reference.
Results and Printout Controls	Lets you select or create an ANSYS Structural Output modeling object to define output.Select an existing modeling object from the list or click Create Modeling Object to create a new one.Click Modify Selected to edit the selected modeling objectFor more information, see ANSYS Structural Output Requests dialog box.	Modal Flexible Body

Output Controls page

Option	Description	Supported solution types	ANSYS Command
Alternative Output Controls	Controls whether you define the output options for the analysis as a modeling object.	All solutions except for Modal Flexible Body.	N/A
Results item (OUTRES,Item)	Controls the solution data written to the output database.	All solutions	OUTRES,ALLOUTRES,BASICOUTRES,NSOLOUTRES,RSOLOUTRES,ESOLSee the ANSYS Commands Reference
Solutions output frequency (OUTPR,,Freq)	Controls the frequency data written to the output file.	All solutions	OUTPR,,FreqSee the ANSYS Commands Reference
Default Frequency (OUTPR,,Freq)	Controls the frequency data written to the output file.	All solutions	OUTPR,,FreqSee the ANSYS Commands Reference

Solution controls page

Option	Description	Supported solution types	ANSYS Command
SOLCONTROL
Key 1 (Optimized defaults activation)	Controls whether the software uses the ANSYS optimized defaults for nonlinear analysis.	Nonlinear Statics	SOLCONTROL, Key 1See the ANSYS Commands Reference
Key 2 (Check contact state)		Nonlinear Statics	SOLCONTROL, Key 2See the ANSYS Commands Reference
Key 3 (Pressure load stiffness)		Nonlinear Statics	SOLCONTROL, Key 3See the ANSYS Commands Reference
Vtol (Tolerance for volumetric compatibility check		Nonlinear Statics	SOLCONTROL, VtolSee the ANSYS Commands Reference
NEQIT
User Specified	Controls whether you can specify a value for the Maximum number of equilibrium equations option.	Nonlinear Statics	NEQITSee the ANSYS Commands Reference
Maximum number of equilibrium equations	Controls the maximum number of equilibrium iterations allowed in each substep.	Nonlinear Statics	NEQITSee the ANSYS Commands Reference

Transient Options page

Option	Description	Supported solution types	ANSYS Command
Mass Damping Coefficient (ALPHAD)	Defines the mass matrix multiplier, α, for damping.	Transient Dynamic-Full MethodTransient Dynamic-Mode Superposition	ALPHADSee the ANSYS Commands Reference
Stiffness Damping Coefficient (BETAD)	Defines the stiffness matrix multiplier, β, in the damping expression specified in the Mass Damping Coefficient (ALPHAD) box.	Transient Dynamic-Full MethodTransient Dynamic-Mode Superposition	BETADSee the ANSYS Commands Reference
Transient Analysis Options (TRNOPT)	Specifies the solution method for the transient analysis.(FULL) Full methodApplies the full method.(VT) Variational technologyApplies the variational technology method.	Transient Dynamic-Full Method	TRNOPTSee the ANSYS Commands Reference
Time Integration Method	Specifies the integration method for the transient analysis.(NMK) Newmark algorithmApplies the Newmark algorithm.HHT algorithmApplies the HHT algorithm.	Transient Dynamic-Full Method	TRNOPT, TINTOPTSee the ANSYS Commands Reference
Time Integration Parameters	Lets you define the transient integration parameters.	Transient Dynamic-Full MethodTransient Dynamic-Mode Superposition	TINTPSee the ANSYS Commands Reference
Amplitude Decay (GAMMA)	Sets the amplitude decay factor for second order transient integration,	Transient Dynamic-Full MethodTransient Dynamic-Mode Superposition	TINTP, GAMMASee the ANSYS Commands Reference
Second Order Parameter (ALPHA)	Sets the second order transient integration parameter. This option is used only if Amplitude Decay (GAMMA) is not specified.	Transient Dynamic-Full MethodTransient Dynamic-Mode Superposition	TINTP, ALPHASee the ANSYS Commands Reference
Second Order Parameter (BETA)	Sets the second order transient integration parameter. This option is used only if Amplitude Decay (GAMMA) is not specified.	Transient Dynamic-Full MethodTransient Dynamic-Mode Superposition	TINTP, DELTASee the ANSYS Commands Reference
First Order Parameter (THETA)	Sets the first order transient integration parameter	Transient Dynamic-Full MethodTransient Dynamic-Mode Superposition	TINTP, THETASee the ANSYS Commands Reference
Oscillation Limit Criterion (OSLM)	Sets the oscillation limit criterion for automatic time stepping of 1st order transients.	Transient Dynamic-Full MethodTransient Dynamic-Mode Superposition	TINTP, OSLMSee the ANSYS Commands Reference
Tolerance Applied to OSLM (TOL)	Sets the OSLM tolerance value.	Transient Dynamic-Full MethodTransient Dynamic-Mode Superposition	TINTP, TOLSee the ANSYS Commands Reference
Smooth Flag Option (AVSMOOTH)	Controls whether or not ANSYS smooths the initial velocity (first order system) or initial acceleration (second order system).	Transient Dynamic-Full MethodTransient Dynamic-Mode Superposition	TINTP, AVSMOOTHSee the ANSYS Commands Reference
Interpolation Factor in HHT algorithm for force and damping terms (ALPHAF)	Sets the Interpolation factor that ANSYS uses in the HHT algorithm for force and damping terms. This option is used only if Amplitude Decay (GAMMA) is not specified.	Transient Dynamic-Full MethodTransient Dynamic-Mode Superposition	TINTP, ALPHAFSee the ANSYS Commands Reference
Interpolation Factor in HHT algorithm for initial term (ALPHAM)	Sets the interpolation factor that ANSYS uses in the HHT algorithm for the inertial term. This option is used only if Amplitude Decay (GAMMA) is not specified.	Transient Dynamic-Full MethodTransient Dynamic-Mode Superposition	TINTP, ALPHAMSee the ANSYS Commands Reference

User Defined Text page

Option	Description	Supported solution types
Insert User Defined Text Before/After
Pre/Post Header**/ASSIGN Commands*FE Model Creation All (CSYS, Nodes, Materials, Elements)GroupsConstraints*Solution**	Lets you specify a User Defined Text modeling object to insert at specific locations in the input file.	All Solutions
Remove Commands Created by Pre/Post When User Defined Text Exists	Controls whether this software removes any commands created by Pre/Post when you insert a User Defined Text modeling object.Select this check box to delete any related commands generated by this software when you insert user defined text. For example, if you insert a User Defined Text modeling object in the materials section of the input file, the software deletes any materials commands generated by Pre/Post.Clear this check box to retain any related commands generated by this software when you insert user defined text. For example, if you insert a User Defined Text modeling object in the materials section of the input file, the software adds the user defined text to the materials commands generated by Pre/Post.	All Solutions

Cyclic Symmetry page (Linear Statics, Modal, Nonlinear Statics, Harmonic - Mode Superposition solutions)

Option	Description
Cyclic Attributes (CYCLIC)	Lets you specify a Cyclic Attributes modeling object to define the number of sectors, the sector angle, and specify the pairs of nodes that the software uses to optionally generate cyclic constraint equations.For more information, see Cyclic symmetry analysis in ANSYS.
Cyclic Options (CYCOPT)	Lets you specify a Cyclic Options modeling object to define options for the solution. For example, you can adjust tolerance values, control the harmonic solution index ranges, and specify whether to manually apply nodal rotations.For more information, see Cyclic symmetry analysis in ANSYS.

Restart page (Modal solutions)

Option	Description
ANSYS Restart	Indicates that you want to restart the analysis after the initial solve completes.
File name from previous run to extract 'jobname' for restart (/FILNAME.jobname)	Lets you specify the name of the results file from the initial solve. ANSYS restarts the analysis from these results.
Linear perturbation options (PERTURB)	Lets you specify a Linear Perturbation Options (PERTURB) modeling object to define the perturbation options for the analysis to restart, such as the analysis type, material behavior, contact status of all contact elements, and the load values to retain in the restart process.For more information, see Specifying linear perturbation options.
Contact element KEYOPTS modification (CNKMOD)	Lets you specify a Contact Element KEYOPTS Modification (CNKMOD) modeling object to modify the contact status for individual pairs of contact elements and the units of normal contact stiffness.For more information, see Modifying the behavior of contact pairs.
Multiframe Restart Parameters (ANTYPE, MODAL, RESTART...)
**Define loadstep at which restart begins (LDSTEP)**Specify loadstep number (found in Jobname.Rnnn)	Lets you specify the load step at which to begin the restart analysis. In a multiframe restart, you can save analysis information at many substeps during the solve and then restart the solve from one of those substeps.
**Define substep at which restart begins (SUBSTEP)**Specify substep number	Lets you specify the solution substep at which to begin the restart analysis.
Specify the manner of a restart (Action)	Controls how ANSYS performs the multiframe restart.(PERTURB) Linear perturbation at restartThe software performs a linear perturbation analysis (MODAL) at the specified loadstep and substep.(CONTINUE) Continue based on specified loadstep and substepThe software continues the analysis based from the specified load step and substep. ANSYS continues the current load step. If that load step ends in the .Rnnn file, the software starts a new load step. (ENDSTEP) Force specified load step to the end of specified substep The software forces the specified load step to end at the specified substep even though the software has not reached the end of the load step. At the end of the specified substep, ANSYS scales ANSYS scales all loads to the level of the current end and stores them in the .LDHI file. A solve that follows this end step starts a new load step.(RSTCREATE) Retrieve information to be written to the results fileAt the restart, the software retrieves information to write to the results file for the specified load step and substep.
Subsequent linear perturbation will be performed	Controls whether ANSYS performs a subsequent linear perturbation analysis.YESSpecifies the first linear static analysis with a subsequent linear perturbation analysis. NOANSYS does not perform a subsequent linear perturbation analysis.

Restart Controls page (Nonlinear Statics solutions)

Option	Description
Restart Controls (RESCONTROLS)	Lets you specify a Cyclic Attributes modeling object to define the number of sectors, the sector angle, and specify the pairs of nodes that the software uses to optionally generate cyclic constraint equations.

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 (ANSYS), 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 } });