Solution Step dialog box (ANSYS)

Option	Description	Supported solutions	ANSYS Command
Description	Opens an editor that lets you enter a description for the step.	All solutions	-
Boundary Condition Control Variables
Evaluation Time	Specifies the value used to evaluate a time-, frequency-, or temperature-dependent boundary condition when you use the boundary condition in a solution that does not support dependent boundary conditions.The software first uses the field evaluation value for the step or subcase to determine the loading value. If no field evaluation value is defined for the step or subcase, the software uses the field evaluation value for the solution.	Linear StaticsNonlinear StaticsThermal	-
Evaluation Frequency	Linear StaticsNonlinear Statics	-
Step-Buckling Method
Description	Opens an editor that lets you enter a description for the step.	Buckling	-
Modes Extraction Method	Specifies the mode extraction method to use.	Buckling	MODOPT, Method
Eigenvalue Generation	Controls whether you specify only the number of modes to generate or the number of modes and the frequency range.	Buckling	-
Number of Modes	Specifies the number of modes to extract for the step.	Buckling	MODOPT, NMODE
Eigenvalue Range-Lower Limit	Specifies the beginning (lower end) of the frequency range.	Buckling	MODOPT, FREQB
Eigenvalue Range-Upper Limit	Specifies the ending (upper end) of the frequency range.	Buckling	MODOPT, FREQE
Properties
Phase Angle (to define imaginary VALUE2)	Defines the amount of time by which a load lags or leads a frame of reference.	Harmonic Full MethodHarmonic Mode Superposition	VALUE2 field

General options

Option	Description	Supported solution types	ANSYS command
Properties
Temperature Pre-Load Type	Applies temperatures from the results of a thermal analysis as loads in a structural analysis. Select an option from the list to identify the type of source file for the results.	Linear StaticsNonlinear Statics	BFFor more information, see the ANSYS Commands Reference manual.
Nastran Pre-Load Results FileSimcenter 3D Thermal Pre-Load Results FileAbaqus Pre-Load Results File****ANSYS Pre-Load Results File	Lets you specify the name and location of the results file to use.	Linear StaticsNonlinear Statics	BFFor more information, see the ANSYS Commands Reference manual.
Force Pre-Load Type	Applies temperatures from the results of a thermal analysis as loads in a structural analysis. Select an option from the list to identify the type of source file for the results.	Linear StaticsNonlinear Statics	BFFor more information, see the ANSYS Commands Reference manual.
Simcenter 3D Flow Pre-Load Results File	Applies pressures and shear forces from the results of Simcenter 3D Flow analysis as loads in a structural analysis. Select an option from the list to identify the type of source file for the results.	Linear StaticsNonlinear Statics	BFFor more information, see the ANSYS Commands Reference manual.
Change Step Parameters	Controls whether you can change the parameters within the step.	Nonlinear Statics	-
Time at The End of Step (TIME)	Specifies the time at the end of the load step.	Nonlinear Statics	TIMEFor more information, see the ANSYS Commands Reference manual.
NSUBST
Number of Substeps (NBSTP)	Specifies the number of substeps for this load step. This defines either the time step size or the frequency increment.	Nonlinear Statics	BFFor more information, see the ANSYS Commands Reference manual.
**Minimum Number of Substeps (NSBMN)**Maximum Number of Substeps (NSBM)	Specifies the minimumand maximum number of substeps for this load stope.	Nonlinear Statics	-

Output controls page options

Option	Description	Supported solution types	ANSYS command
Change output controls	When selected, enables you to modify the output controls for the step.Clear this check box to use the output controls defined for the solution.	Linear StaticsNonlinear Statics	N/A
Alternative Output Controls	Controls whether you define the output options for the step as a modeling object.	All solutions except for Modal Flexible Body.	N/A
Output controls→Results file (OUTRES)
Results item (OUTRES,Item)		Linear StaticsNonlinear Statics	OUTRES,ALLOUTRES,BASICOUTRES,NSOLOUTRES,RSOLOUTRES,ESOLFor more information, see the ANSYS Commands Reference manual.
Solutions output frequency (OUTRES,,Freq)		Linear StaticsNonlinear Statics	OUTRES,,FreqFor more information, see the ANSYS Commands Reference manual.
Default Frequency (OUTRES,,Freq)		Linear StaticsNonlinear Statics	OUTRES,,FreqFor more information, see the ANSYS Commands Reference manual.
Output controls→Solution Printout (OUTPR)
Same as Results file	When selected, sets the solution printout options to be the same as the results file options.	Linear StaticsNonlinear Statics	-
Results item (OUTPR,Item)		Linear StaticsNonlinear Statics	OUTPR,BASICOUTPR,NSOLOUTPR,RSOLOUTPR,ESOLOUTPR,NLOADOUTPR,VENGOUTPR,ALLFor more information, see the ANSYS Commands Reference manual.
Solutions output frequency (OUTPR,,Freq)	Controls at which substeps the software writes the solution results you selected from theResults item list.NONE: Suppresses the writing of the specified results for all substeps.ALL: Writes the specified results for all substeps.LAST: Writes the specified results only for the last substep for each step.Specify: Lets you write the specified results at every nth substep as well as the last substep, where n is the value you enter in the Default Frequency box.	Linear StaticsNonlinear Statics	OUTPR,,FreqFor more information, see the ANSYS Commands Reference manual.
Default Frequency (OUTPR,,Freq)	If you select Specify from the Solution output frequency list, lets you specify that you want to write the results at every nth substep where n is the value you enter here.	Linear StaticsNonlinear Statics	OUTPR,,Freq, nFor more information, see the ANSYS Commands Reference manual.

Contact options (Available for steps in Nonlinear Statics analyses only)

Change Normal Penalty Stiffness (FKN)
Change Normal Penalty Stiffness	Select this check box to modify the value of the normal penalty (contact) stiffness (FKN real constant) in this step.For certain contact problems, you may choose to use the real constant FKN to define a normal contact stiffness factor. The usual factor range is from 0.01-1.0, with a default of 1.0. The default value is appropriate for bulk deformation. If bending deformation dominates, you should use a smaller value (0.1). For more information, see the ANSYS Contact Technology Guide.
New Value	Specify the value to use for the FKN real constant in this step.
Applied to all Regions	Select this option to apply the new FKN value to all regions in the model.
Select a Region	Select this option to apply the new FKN value only to selected regions.
Change Penetration Tolerance (FTOLN)
Change Penetration Tolerance	Select this check box to modify the penetration tolerance in this step.When you are using the Augmented Lagrangian contact algorithm, the software uses the penetration tolerance to calculate the allowable penetration. The typical range for this value is <1.0.For more information, see the ANSYS Contact Technology Guide.
New Value	Specify the value to use for the FTOLN real constant in this step.
Applied to all Regions	Select this option to apply the new FTOLN value to all regions in the model.
Select a Region	Select this option to apply the new FTOLN value only to selected regions.
Change Pinball Region (PINB)
Change Pinball Region	Select this check box to modify the value of the pinball region scaling factor (PINB real constant) in this step.In ANSYS analyses, the pinball region is a contact element parameter that differentiates between far field open and near field open contact status. The pinball region is like a spherical boundary that surrounds each contact detection point. You can use the real constant PINB to define a scaling factor or absolute value for the pinball region.For more information, see the ANSYS Contact Technology Guide.
New Value	Specify the value to use for the PINB real constant in this step.
Applied to all Regions	Select this option to apply the new PINB value to all regions in the model.
Select a Region	Select this option to apply the new PINB value only to selected regions.
Change Contact Opening Stiffness or Contact Damping (FKOP)
Change Contact Opening Stiffness or Contact Damping	Select this check box to modify the contact opening stiffness value or the contact damping coefficient (FKOP real constant) in this step.For the no separation or bonded contact surface interaction model, FKOP is the stiffness factor applied when contact opens.For the standard or rough contact surface interaction models, FKOP is a contact damping coefficient.For more information, see the ANSYS Contact Technology Guide.
New Value	Specify the value to use for the FKOP real constant in this step.
Applied to all Regions	Select this option to apply the new FKOP value to all regions in the model.
Select a Region	Select this option to apply the new FKOP value only to selected regions.

Cumulative Load options

Option	Description	Supported solutions	ANSYS Command
FCUM Command
Forces/Moments in this step will	Controls how the software accumulates force loads.	Linear Statics	FCUM: OperFor more information, see the ANSYS Command Reference manual.
Scale Factor (RFACT)	Lets you specify a scale factor that the software applies to the next load value.	Linear Statics	FCUM: RFACTFor more information, see the ANSYS Command Reference manual.
SFCUM Command
Surface loads in this step will	Controls how the software accumulates surface loads.	Linear Statics	SFCUM: OperFor more information, see the ANSYS Command Reference manual.
Scale Factor (FACT)	Lets you specify a scale factor that the software applies to the next load value.	Linear Statics	SFCUM: FACTFor more information, see the ANSYS Command Reference manual.
BFCUM Command
Body loads in this step will	Controls how the software accumulates nodal body force loads.	Linear Statics	BFCUM: OperFor more information, see the ANSYS Command Reference manual.
Scale Factor (FACT)	Lets you specify a scale factor that the software applies to the next load value.	Linear Statics	BFCUM: FACTFor more information, see the ANSYS Command Reference manual.
Temperature adjustment (TBASE)	Controls the temperature adjustment the software makes when adding or replacing nodal body force loads.	Linear Statics	BFCUM: TBASEFor more information, see the ANSYS Command Reference manual.
BFECUM Command
Surface loads in this step will	Controls how the software accumulates element body loads.	Linear Statics	BFECUM: OperFor more information, see the ANSYS Command Reference manual.
Scale Factor (FACT)	Lets you specify a scale factor that the software applies to the next load value.	Linear Statics	BFECUM: FACTFor more information, see the ANSYS Command Reference manual.

Delete Load page options

Option	Description	Supported solution types	ANSYS Command
DDELE Command
DOF constraints at the end of this step	Controls whether DOF constraints will be kept or deleted at the end of the current load step.	Nonlinear StaticsThermal	DDELEFor more information, see the ANSYS Command Reference manual.
FDELE Command
Forces/Moments at the end of this step	Controls whether forces and moments will be kept or deleted at the end of the current load step.	Linear StaticsNonlinear StaticsThermal	FDELEFor more information, see the ANSYS Command Reference manual.
BFDELE Command
Body Loads at the end of this step	Controls whether body loads will be kept or deleted at the end of the current load step.	Linear StaticsNonlinear StaticsThermal	BFDELEFor more information, see the ANSYS Command Reference manual.
BFEDELE Command
Element body loads at the end of this step	Controls whether element body loads will be kept or deleted at the end of the current load step.	Linear StaticsNonlinear StaticsThermal	BFEDELEFor more information, see the ANSYS Command Reference manual.

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 Step 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 } });