Nonlinear Control Parameters - Global dialog box (Simcenter Nastran)

Use this dialog box to set values for a Nonlinear Control Parameters - Global modeling object for SOL 401 Multi-Step Nonlinear, SOL 402 Multi-Step Nonlinear Kinematics, and SOL 414.

Note:

The options that appear on the dialog box depend on the solution type for which you are creating the modeling object.

Modeling Object
Name	Sets a unique name for the modeling object.
Label	Sets a unique integer 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.
Properties
To add a parameter to the NLCNTLG bulk entry, click Add .To remove a parameter from the NLCNTLG bulk entry, click Remove .
Card Name	Displays the name of the corresponding solver command or keyword.
Solution Applicability View	Specifies the solution type for which you want to set the nonlinear control parameters. When you select a solution type, the dialog box updates to show the options that apply to the selected solution. This option is for display only. If you set SOL 401 options for nonlinear control parameters in a SOL 402 solution, the SOL 401 settings have no effect on the solve.

Global Parameters page (SOLs 401 and 402) / General Parameters tab (SOL 414)

The options that appear depend on the specified solution type.

Option	Description
Solver Type (RESO)	Specifies the linear solver. If you do not select a solver, the software uses the Sparse solver, or the Parallel solver when a DMP parallel computation is requested.SkylineNo pivoting strategy is performed with this method. In rare cases, it can be faster than the Sparse solver for very small problems (less than 5,000 degrees of freedom), but you cannot use it with contact with large displacements (reprofiling). SparseRecommended for almost all problems because it reduces the time and memory required for solving a system of linear equations.ParallelFor distributed-memory parallel (DMP) processing, which executes the MUMPS (MUltifrontal Massively Parallel sparse direct Solver) parallel solver. For more information on the number of instances of the solver that are started, memory size, and so on, see Parallel solver in the Samcef documentation. For more information, see the RESO parameter of the NLCNTLG bulk entry.
Matrix Symmetry (INLY)	Specifies the type of matrix symmetry for nonlinear static, preload, and dynamics subcases.Symmetry ActivatedSelect this option unless you need convergence in special cases. Buckling, normal modes, cyclic normal modes, and Fourier normal modes subcases always use this symmetric solver.Unsymmetry ActivatedSelect this option to improve convergence for contact friction, follower forces, and gyroscopic effects in dynamic analyses. This solver increases computation time because it doubles the number of arithmetic operations of the linear solution. Selecting Unsymmetry Activated forces the solver to use full matrices regardless of whether symmetry exists.When your solution contains complex modes subcases, the software selects Unsymmetry Activated automatically. Complex modes subcases always use the unsymmetric solver.Note: If you want large displacement effects (updated element coordinates and follower forces) to be included in the stiffness matrix, select Unsymmetry Activated, and select the Large Displacements check box in the Solution dialog box (Nastran), Parameters page.For more information, in the Nastran documentation, see the INLY parameter of the NLCNTLG bulk entry and Contact convergence.In the Samcef documentation, see the INLY parameter of the .ALG command and Contact Modeling.
Stiffness Matrix Check when Computation Starts (KINI)	Specifies whether to perform a check of the model's initial stiffness and kinematic modes. The model check does the following:Produces the largest, smallest, and mean diagonal values of the stiffness matrix. If the ratio between the smallest and largest diagonals is greater than 1.E8, numerical problems can occur during the solve. A warning message is printed to the .f06 file at time zero and also during the solve.Finds the degrees of freedom for which the corresponding row and column of the stiffness matrix are equal to 0. Zero can indicate, for example, a degree of freedom that is not connected properly to the structure, an unconnected degree of freedom (that is, a point with mass), a beam stiffness of 0, or a Lagrange multiplier with too many fixations.Removes the degrees of freedom that are not connected and inverts the stiffness matrix. This check identifies degrees of freedom with zero pivots. A zero pivot related to a Lagrange multiplier indicates a redundant constraint (two rigid bodies in parallel). A zero pivot related to a real node corresponds to a kinematic mode, which is subsequently computed. This helps you to verify the boundary conditions. For more information on zero pivots, see Zero/Negative Pivots in the Samcef documentation.Note: This check does not take into account kinematic conditions that are introduced by the Initial Position, Enforced Displacement Constraint, or User Defined Constraint boundary conditions, or by contact conditions.The result of the check appears in the .f06 file. For more information, see the KINI parameter of the Samcef .ALG command.
Initial Static and/or Steady-State Computation (IREF)	Specifies the initial condition of the solve for static computations, steady state, or both.NoneNo initial static or steady state is computed.Initial Static ComputationOnly the initial static state is computed. Steady-State ComputationOnly the steady state is computed. This option applies to subcases of type Subcase - Nonlinear Dynamics. Initial Static and Steady-State ComputationBoth the initial static state and steady state are computed. This option applies to subcases of type Subcase - Nonlinear Dynamics. For more information, see Initial static computation in the Samcef documentation and the IREF parameter of the NLCNTLG bulk entry.
Allow Chocking Behavior (CHOCK)	Appears when Solution Applicability View is set to All Solutions or SOL 401 Multi-Step Nonlinear. Applies to SOL 401 only.Specifies whether you want the solver to use any chocking elements that you added to your model. Chocking elements apply to axisymmetric analyses. For more information, see Chocking elements (SOL 401).
Switch off Plasticity Computation (PLSHSOL)	Specifies whether to turn off plasticity at a Gauss point when the hydrostatic pressure changes sign. Hydrostatic pressure is the portion of the total stress state that changes volume. When the hydrostatic pressure changes sign at any Gauss point and the software turns plasticity off, plasticity remains off at those Gauss points for the rest of the solution. The software retains the plastic strain that occurred up to that time step, and the solution continues using elastic properties at those Gauss points.To turn off the plasticity computation when the hydrostatic pressure changes sign, select Yes. Setting Switch off Plasticity Computation (PLSHSOL) to Yes turns off the plasticity computation for all subcases. To turn on the plasticity computation for individual subcases, set Ignore Plasticity for Pressure Sign Change (PLSHUT) to Yes on the Nonlinear Control Parameters dialog box (SOL 401) or Nonlinear Control Parameters - Subcase dialog box (SOL 402). To retain the plasticity computation even when the hydrostatic pressure changes sign, select No. For more information, see Hydrostatic pressure plasticity switch in Plasticity analysis.
Scaling of Material Properties and Loads for Cyclic Symmetry Groups (CY3DSCL)	Applies to SOL 401 only.Specifies whether to scale elemental mass, stiffness, and applied loads.OnBy default, the software applies scaling automatically if both of the following conditions are detected:2D axisymmetric elements.Cyclic Symmetry dialog box→ Stages group→ Select Elements contains a selection of elements internal to the sector.When both of the above conditions are detected, the software scales elemental mass and stiffness as well as loads applied to the following type of elements selected in the Stages group of the Cyclic Symmetry dialog box:CHEXACTETRACPENTACPYRAMCONMi (Mass only)OffDisables automatic scaling.Note: The software scales elemental mass, stiffness, and applied loads using the calculated number of segments (NSEG) as a scaling factor, which is calculated automatically.For more information, see the CY3DSCL parameter of the NLCNTL bulk entry.

Advanced Parameters page (SOLs 401 and 402) / Additional Parameters tab (SOL 414)

The options that appear depend on the specified solution type.

Option	Description
Solver Version for Previous Algorithm Behavior (MODEVERS)	Applies to SOL 402, SOL 414,103, and SOL 414,129.Sets the Simcenter 3D version number to a previous version. This forces the solver to use the defaults and algorithms of the specified release. For example, if a model quickly converges in Simcenter 3D 2019.1 but not in Simcenter 3D 2019.2, you can set this value to 20191. The version number must be an integer with no decimal point.For releases prior to Simcenter 3D 2019.1, you can enter Samcef release numbers, such as 19, 18, 17, and so on.The default for this option is always the current version.
Number of Kinematic Modes to Save as Output (NKINE)	Applies to SOL 402, SOL 414,103, and SOL 414,129.Sets the maximum number of kinematic modes that you want to save to the results file. The kinematic modes correspond to models that move or rotate, such as models that are configured with kinematic boundary conditions. The default is to save 10 modes.For information on kinematic boundary conditions, see Kinematic Driver boundary condition and Joint Time Constraint boundary condition.
Threshold to Detect Zero Pivots (PRECPIVO)	Applies to SOL 402, SOL 414,103, and SOL 414,129.Sets the threshold to consider a small stiffness as a numerical zero (default = 1e-08) on the diagonal of the stiffness matrix. For information on zero pivots, see the Stiffness Matrix Check when Computation Starts (KINI) global parameter or Zero/Negative Pivots in the Samcef documentation.
Stress-Strain Conversion Method (STRCONV)	Applies to SOL 401 and SOL 402.Specifies how you want the solver to convert stress-strain curves.Exact MethodTypeConversionEngineering strain → log (true) strain Engineering stress → true stressStandard MethodThe standard method assumes a Poisson's ratio of 0.5 for the plastic part.TypeConversionEngineering strain → log (true) strain Engineering stress → true stresswhere:εT = engineering total strainεe = engineering elastic strainεp = engineering plastic strainS = engineering stressv = Poisson’s ratioσ = true stressεl = log (true) strainE = Young's modulusFor more information, see SOL 401 and 402 - Stress-strain measures in the Simcenter Nastran in the Multi-Step Nonlinear User’s Guide (SOL 401 and SOL 402).	Type	Conversion	Engineering strain → log (true) strain		Engineering stress → true stress		Type	Conversion	Engineering strain → log (true) strain		Engineering stress → true stress
Type	Conversion
Engineering strain → log (true) strain
Engineering stress → true stress
Type	Conversion
Engineering strain → log (true) strain
Engineering stress → true stress
Bolt Preload Method (BOLTMETH)	Applies to SOL 402.Specifies the method for connecting the faces on the two cut parts for the following types of Bolt Pre-Load:Force or Displacement on 3D Elements - Cut Plane (ETYPE=2)Force or Displacement on 2D Solid Elements - Cut Plane (ETYPE=2)For SOL 402, these types of bolts can be modeled with 2D axisymmetric, plane stress, and 3D elements.RBE3 Elements and Sensor along the CutCreates the contact using an RBE3 element on each face of the bolt cut. Both RBE3 elements are connected using one 3D Sensor element (SE3D) to apply the preload. The preload is applied to the sensor element in the direction that you define for the bolt.For more information, see 3D Sensor element (SE3D) in the Simcenter Samcef documentation.Contact Elements along the CutCreates contact between the two faces of the bolt cut. The contact is created with infinite friction so that no sliding can occur. The preload is applied by varying the penetration of the contact. The bolt orientation is always perpendicular to the cut.If you omit a value for Bolt Preload Method (BOLTMETH), the solver determines the method as follows:If you defined the bolt preload coordinate system as global or Cartesian, the solver models the bolts using the RBE3 Elements and Sensor along the Cut method.If you defined the bolt preload coordinate system as automatic, the solver models the bolts using the Contact Elements along the Cut method.Note: When you select a method, all bolts are modeled using that method regardless of the type of coordinate system used to define them.
Fourier Harmonics Method (FHMETH)	Applies to SOL 402.Specifies how to couple the stiffness contribution from harmonics shape functions, and which harmonics to consider — only the positive harmonics, or both the positive and negative harmonics. Uncoupling the matrices or considering only one direction of the harmonics can lead to quicker solving time per iteration because fewer terms are considered in the matrices. However, more iterations might be needed to reach the equilibrium.When your analysis contains nonlinear conditions (material nonlinearity, large displacements, large strain, or contact), coupled harmonics become more important to achieve convergence. Some nonlinear problems can still converge with the uncoupled option, but the number of iterations may increase. However, the results of a converged coupled analysis or a converged uncoupled analysis are the same.When your analysis is linear, uncoupling the matrices improves performance.When your analysis includes normal modes subcases, you can use the Positive Harmonics Only options to omit duplicate modes. Omitting the negative harmonics reduces the model size, but you must fully understand the loading and resulting deformations for your analysis to ensure that the negative harmonics are not necessary in the results.Coupled HarmonicsFully couples the harmonics of one matrix to the other matrix. Computes zero, positive, and negative harmonics.Uncoupled HarmonicsDecouples the matrices. Computes zero, positive, and negative harmonics.Decoupling the matrices creates fewer terms in the matrix, so the results are less accurate than for coupled matrices, but the solution solves more quickly. (Newton-Raphson allows the solution to still converge.) However, if your solution does not converge with Uncoupled Harmonics, try setting Fourier Harmonics Method (FHMETH) to Coupled Harmonics.This option is suitable for linear analyses, and it allows the solution to solve more quickly.Harmonics Coupled by PairsFor composites applications. Couples the positive and negative pairs of harmonics, and computes the zero, positive, and negative harmonics.Coupled Harmonics - Positive Harmonics OnlyCouples the zero and positive harmonics, and computes the zero and positive harmonics.Uncoupled Harmonics - Positive Harmonics OnlyUncouples the zero and positive harmonics, and computes the zero and positive harmonics.Harmonics Coupled by Pairs - Positive Harmonics OnlyPerforms the same coupling and computation as Uncoupled Harmonics - Positive Harmonics Only.For more information, see the FHMETH parameter of the NLCNTLG bulk entry.

Restart Parameters page (SOLs 401 and 402) / Additional Parameters tab (SOL 414)

The options that appear depend on the specified solution type.

For SOL 414, use this tab to enable the Generate Restart Point (RSTGEN) option.

For SOLs 401 and 402:

• Use the options on the Restart Management page in the Solution dialog box to set options for generating and using a restart file. From the Restart Management page, you can select the restart file and the subcases in the file.

• Use the options on the Restart Parameters page in this dialog box when you need to temporarily override a restart setting or when you need to change the unit number of the initial run file. The settings on the Restart Parameters page override over those on the Restart Management page.

Option	Description
Generate Restart Point (RSTGEN)	For SOL 414, specifies whether to save the results files necessary to recover results using the Results Recombination (for 2D axisymmetric and 3D structures coupled with the Fourier Multi Harmonic and 3D Coupling simulation object) and Superelement Recovery commands. For SOLs 401 and 402, specifies whether to save results and restart points to use in a restart solution. This data is saved at the end of the subcase or at the last converged time step for each static, dynamic, and preload subcase.Select Yes if this is the initial run solution or if this is the restart run of a solution that you also want to use as an initial run. For SOL 401, the data is saved in the .op2 file.For SOL 402, the data is saved in the .op2, .sdb, .adb, and .u18 files.Select No if this is the restart run. The solver does not save restart data.
Unit Number of Initial Run to Restart from (RSTUNIT)	Sets the unit number that identifies the .op2 file you are using for the restart run. In most cases, leave this value at its default of 161. If you need to use a different unit number, we recommend that you use a number greater than 161 to avoid potential conflicts. However, you can use any number.This option is available for rare cases when this number conflicts with your own numbering system. For example, you may have manipulated files in DMAP using the ALTER executive control statement. The unit number is used in the ASSIGN statement in the File Management section of the Nastran input file.
Subcase ID of Initial Run to Restart from (RSTFROM)	Sets the subcase in the initial run whose results you want to use to start the restart run. To identify the subcase IDs and the time steps that you want to use, view the initial run results in the Post Processing Navigator. The Post Processing Navigator organizes the results according to subcase ID and time step.
Subcase ID of in Restart Run (EXEFROM)	Specifies the subcase from which you want the restart run to start. This subcase can be the same as the subcase you set in Subcase ID of Initial Run to Restart from (RSTFROM), or it can be a new one in the restart solution.If you do not specify a subcase, the restart run starts with the subcase you selected from the Subcase ID of Initial Run to Restart from (RSTFROM) list.Note: The subcase you select must be sequentially dependent.
Model Validation for Restart Run (MDLVAL)	Specifies whether to compare the model data in the initial run .op2 file to the current model data. In general, the models should match. Sometimes, however, you may need to modify the model to ensure convergence. For example, you may need to add a spring connection. If you do that, select No. Otherwise, the solution will not run.For information on the changes you can make in the restart run solution, see External restarts.

Obsolete Parameters page

The Obsolete Parameters page lists parameters that are no longer supported in Simcenter Nastran. If you specify a parameter, Pre/Post writes the parameter to the Nastran input file and issues a warning message to indicate that the parameter is obsolete.

Option	Description
Stress-Strain Measure for All Material Laws (STRMEAS)	Note: This is an advanced option that is intended only for special cases. This parameter is no longer supported as of the Simcenter Nastran 2020.2 release. Specifies how you want the solver to calculate stress-strain. The stress-strain measure you select here overrides the stress-strain measure that is defined by your setting for Large Strains (LGSTRN) on the Solution dialog box.Note: This option is ignored for materials that support the Kirchhoff stress-strain measure, such as hyperelastic materials.*Green Strain, PK2 Stress***Log Strain, Cauchy Stress (True)****Biot Strain, Biot Stress (Engineering)**Log Strain, Kirchhoff StressThe option you select also determines how results are saved in the output.For more information, see SOL 401 and 402 - Stress-strain measures in the Simcenter Nastran in the Multi-Step Nonlinear User’s Guide (SOL 401 and SOL 402).
Output Label for Element Stress-Strain Measures (STROUT)	Specifies how you want stress and total strain element measures to be labeled in post processing views. The computation in the material law is done using your selection for Large Strains (LGSTRN) (or the Stress-Strain Measure for All Material Laws (STRMEAS) advanced option). Thus, you can use Output Label for Element Stress-Strain Measures (STROUT) to convert the stress and total strain results to a different measure for output. Other results, such as plastic strain, thermal strain, and so on, cannot be converted to a measure other than the one used in the selected material law.Note: If you used the advanced Stress-Strain Measure for All Material Laws (STRMEAS) option, we recommend that you select the same value for Stress-Strain Measure for All Material Laws (STRMEAS) and Output Label for Element Stress-Strain Measures (STROUT).*Green Strain, PK2 Stress***Log Strain, Cauchy Stress (True)****Biot Strain, Biot Stress (Engineering)**Log Strain, Kirchhoff StressThis parameter does not affect the results that are saved inside material routines, such as plastic strain or creep strain. Those results adhere to your selection for Large Strains (LGSTRN) (or the Stress-Strain Measure for All Material Laws (STRMEAS) advanced option).

Learn more

SOL 402 Multi-Step Nonlinear Kinematics

SOL 402 Multi-Step Nonlinear Kinematics workflow

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Nonlinear Control Parameters - Global dialog box (Simcenter Nastran), 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 } });