Nonlinear Control Parameters dialog box (Simcenter Nastran SOL 401/Simcenter 3D Multiphysics)

For more information about the options in this dialog box, see the NLCNTL bulk data entry in the Simcenter Nastran Quick Reference Guide.

To add a parameter to your solution, specify the appropriate value and click Add .

General Convergence and Iteration Control

Convergence Criteria (CONV)	Lets you specify the criterion to use for convergence, such as displacement (U).
Error Tolerance for Load (EPSP)	If you select Load from the Convergence Criteria (CONV) list, specify the load (P) error tolerance.
Error Tolerance for Displacement (EPSU)	If you select Displacement from the Convergence Criteria (CONV) list, specify the displacement (U) error tolerance.
Error Tolerance for Work (EPSW)	If you select Work from the Convergence Criteria (CONV) list, specify the work (W) error tolerance.
Fluid Penetration Pressure Update (FPPUPDT)	Specifies when the software updates the fluid pressure defined with the Fluid Penetration Pressure load. At the Beginning of Every Time StepThe fluid pressure application is updated only at the beginning of every time step using the final contact status from the previous time step. For the first time step when no previous contact status exists, the fluid pressure is not applied to any elements, including elements that are not in a contact region. This option requires that you include enough time steps for the coupled contact and fluid pressure to become established and achieve a steady state.For All Iterations in a Time StepThe fluid pressure is updated for every solution iteration that occurs in a single time step. This option keeps the fluid pressure current with the changing contact status, but it requires more computation time and can cause contact convergence issues if the fluid pressure and the contact conditions are strongly coupled
Maximum Bisections (MAXBIS)	Lets you define the maximum number of bisections allowed for each load increment.
Maximum Diverging Conditions (MAXDIV)	Lets you specify the limit on probable divergence conditions per iteration before the software assumes that the solution diverges.
Maximum Iterations per Time Step (MAXITER)	Specifies the maximum number of iterations in each time step.
Maximum Quasi-Newton Vectors (MAXQN)	Lets you specify the maximum number of quasi-Newton correction vectors to save in the database.
Norm for Force Criterion (NORMP)	Lets you specify the norm criteria for the force convergence error function.
Norm for Displacement Criterion (NORMU)	Lets you specify the norm criteria for the displacement convergence error function.
Reference Value for Force Criterion (REFP)	(Optional) Replaces the denominator in the force convergence error function with this value.
Reference Value for Displacement Criterion (REFU)	(Optional) Replaces the denominator in the displacement convergence error function with this value.

Bolt Preload

Error Tolerance on Bolt Preload Force (EPSBOLT)	Defines the convergence tolerance for non-zero preloads. If the difference between the preload that Nastran computes and the preload that you define is less than this value, then the software considers the bolt preload calculation to have converged.
Maximum Number of Bolt Iterations (ITRBOLT)	Specifies the maximum number of bolt iterations before the software considers the bolt preload calculation to have failed to converge.
Bolt Scale Parameters (MISFBLT)	Limits the bolt strain from one preload increment to the next.
Bolt Diagnostic Level (MSGLVLB)	Controls the diagnostic information that the software generates for bolt calculations.
Tolerance for Zero Bolt Preload (ZERBOLT)	Defines the convergence tolerance for-zero preloads.

General Solution

Time Unassigned Mechanical Load Ramping (LVAR)	Specifies whether time unassigned loads are ramped or stepped.
Diagnostic Level (MSGLVL)	Controls the diagnostic information that the software generates.
Solver	Specifies the solver to use.To use the sparse direct solver, select SPARSE. This solver is robust and reliable and is well-suited to sparse models where you need accuracy.To use the element iterative solver, select ELEMITER. This solver performs well with models that are predominantly comprised of solid elements. This solver may provide faster results but with slightly lower accuracy.To use the hybrid direct-iterative solver, select PARADISO.To use the Multifrontal Massively Parallel sparse direct solver, select MUMPS. This solver is useful for solving large problems on a small number of processors or very large problems in parallel on shared memory or distributed memory machines.
Thermal Strain Loading (THRMST)	Specifies whether to include thermal strain loading in a static solution.
Time Unassigned Temperature Loads Control (TVAR)	Specifies whether time unassigned loads are either ramped or stepped.To have the software gradually increase the value of the temperature load from the final temperature defined for the previous static step to the temperature defined for the current step, select Ramped. The software uses the total number of time increments specified for the step to determine increments at which to increase the temperature.Note: If the previous step does not include a Temperature load, the software gradually increases the temperature from the specified Initial Temperature to the value of the Temperature load in the current step.To have the software apply the full value of the temperature load in the first step, select Stepped. The temperature then remains constant across the step.
Mechanical Loads Control (LOADOFF)	Allows you to include or exclude specific types of mechanical loads.
Viscous Analysis Inertia (INERTIA)	Allows you to optionally turn off the inertial effects for a dynamic subcase.
Initial Acceleration Computation (INACCN)	Controls whether the software computes an initial acceleration value when the first subcase in the solution is a dynamics subcase, or when a dynamic subcase follows a linear statics or pre-load subcase.
Inertia Force Scaling for RFORCE and RFORCE1 (RFVAR)	Controls how the software interpolates the time variation for the rotational loads.

Stiffness Control

Follower Stiffness (FOLLOWK)	Includes follower stiffness from follower loads defined with force or pressure loads (FORCE1, FORCE2, PLOAD, or PLOAD4 bulk data entries).
Stiffness Update Strategy (KUPDATE)	Specifies the stiffness update strategy.To use the initial stiffness approach, type -1.To use the automatic stiffness update (full Newton-Raphson), type 0.To use a Quasi Newton-Raphson approach, specify a value greater than 1. The number you specify is the number of iterations before a stiffness update.
Spin Softening (SPINK)	Controls whether spin softening is included in the solution.
Material Stiffness Matrix Option (STFOPTN)	Specifies the stiffness matrix to use.To use the elastic stiffness matrix, select Elastic.To use the tangent stiffness matrix, select Tangent.To use the elastic stiffness matrix to start each step and the tangent stiffness matrix at any intermediate stiffness update, select Elastic and Tangent.
Stress Stiffening (STRESSK)	Controls whether stress stiffening is included in the solution.
Update Stiffness at Beginning of Time Step (TSTEPK)	Controls whether the software updates the stiffness at the beginning of each time step.
Stiffness Matrix Stabilization (MSTAB)	Lets you control whether the software uses the stiffness matrix stabilization option.
Matrix Stabilization Factor (MSFAC)	Lets you specify the matrix stabilization factor to use (specify a real number).
Tangential Contact Stiffness in Linear Perturbation Subcase (KMODTN)	Specifies how tangential contact stiffness (friction) from a nonlinear subcase (Preload, Nonlinear Statics, and Nonlinear Dynamics) is applied to a sequentially dependent modal subcase (Normal Modes, Cyclic Modes, and Axisymmetric Fourier Modes). For example, if your analysis includes a nonlinear subcase that requires frictionless contact, but it is followed by a sequentially dependent modal subcase that requires tangential stiffness, use this option to select the type of friction to apply to the modal subcase.Each option lets you independently control how the stiffness is applied from contact pairs that are defined with friction (Frictional Contact) and contact pairs that use no friction (Frictionless Contact). Frictional Contact: Sticking Stiffness; Frictionless Contact: No Stiffness (Default)Frictional Contact: Sticking Stiffness—Applies a uniform frictional contact stiffness of (0.1 * normal stiffness) to the modal subcase.Frictionless Contact: No Stiffness—Applies no frictional stiffness to the modal subcase.Frictional Contact: Sticking and Sliding Stiffnesses; Frictionless Contact: No Stiffness****Frictional Contact: Sticking and Sliding Stiffnesses—Applies the final tangential contact stiffness from the end of the preceding nonlinear subcase to the modal subcase. The applied tangential contact stiffness can be a mixture of sticking and sliding stiffness values.Frictionless Contact: No Stiffness—Applies no frictional stiffness to the modal subcase.Frictional Contact: Sticking and Sliding Stiffnesses; Frictionless Contact: Sticking Stiffnesses****Frictional Contact: Sticking and Sliding Stiffnesses—Applies the final tangential contact stiffness from the end of the preceding nonlinear subcase to the modal subcase. The applied tangential contact stiffness can be a mixture of sticking and sliding stiffness values.Frictionless Contact: Sticking Stiffness—Applies a uniform frictional contact stiffness of (0.1 * normal stiffness) to the modal subcase.Frictional Contact: Sticking Stiffness; Frictionless Contact: Sticking Stiffness****Frictional Contact: Sticking Stiffness—Applies a uniform frictional contact stiffness of (0.1 * normal stiffness) to the modal subcase.Frictionless Contact: Sticking Stiffness—Applies a uniform frictional contact stiffness of (0.1 * normal stiffness) to the modal subcase.Note: You can define Tangential Contact Stiffness in Linear Perturbation Subcase (KMODTN) in a Nonlinear Control Parameters modeling object at the subcase level. This allows you to assign a different Tangential Contact Stiffness in Linear Perturbation Subcase (KMODTN) value to each modal subcase.For more information, see the KMODTN parameter of the Simcenter Nastran NLCNTL bulk entry.

Contact

Number of Permissible Contact Divergences Prior to Bisection (CNTMDIV)	Lets you specify the allowable number of contact divergences before the software initiates bisection.
Friction Coefficient Threshold for Asymmetric Stiffness Generation (FSMTOL)	Defines the contact friction coefficient threshold that controls whether the sliding contact stiffness includes the unsymmetric stiffness terms. Specify a real number ≥ 0.0.
Asymmetric Stiffness Generation (KSYM)	When the software generates an unsymmetric material stiffness, controls to symmetrize the unsymmetric matrix.
Global Stiffness Symmetrization Tolerance (KSYMTOL)	Specifies the tolerance value for symmetrizing the unsymmetric material global stiffness.
Contact Diagnostic Level (MSGLVLC)	Controls the level of diagnostic output for contact that the software generates.
Asymmetric Solver (USOLVER)	Specifies the unsymmetric solver to use.

Plasticity and Creep Control

Maximum Creep Increment to Elastic Strain Ratio (CRCERAT)	Specifies the ratio of maximum creep increment to elastic strain that the software uses to calculate the next time step.
Maximum Creep Increment (CRCINC)	Specifies the maximum creep increment that the software uses to calculate the next time step. Specify a real value ≥0.0.
Creep Effects (CREEP)	Specifies whether to include creep effects in the solution.
Creep Strain Increment (CRICOFF)	Specifies the creep strain increment below which the next time step is the product of the current time step and the Creep Maximum Time Step Multiplying Factor (CRMFMX) value. Specify a real value that is ≥0.0 and ≤1.0.
Creep Integration Factor (CRINFAC)	Specifies the integration factor that the software uses to calculate incremental creep strain. Specify a real value that is ≥0.0 and ≤1.0.
**Creep Minimum Time Step Multiplying Factor (CRMFMN)**Creep Maximum Time Step Multiplying Factor (CRMFMX)	Specifies the minimum and maximum values by which to multiply the time step. Specify a real value that is ≥0.0 and ≤1.0.
Creep Absolute Truncation Error (CRTEABS)	Defines the maximum absolute truncation error. Specify a real value that is ≥0.0 and ≤1.0.
Crossover Value for Creep Strain (CRTECO)	Specifies the crossover value for creep strain. Specify a real value that is ≥0.0 and ≤1.0.If the creep strain is less than this value, the software uses the Creep Absolute Truncation Error (CRTEABS) value to calculate the creep strain.If the strain is greater than this value, the software uses the Creep Maximum Relative Truncation Error (CRTEREL) value to calculate the creep strain.
Creep Maximum Relative Truncation Error (CRTEREL)	Specifies the maximum relative truncation error. Specify a real value that is ≥0.0 and ≤1.0.
Plasticity Effects (PLASTIC)	Specifies whether to include plasticity effects in the solution.
Maximum Equivalent Plastic Strain Increment (PLLIM)	Sets the maximum equivalent plastic strain that can occur in a time step (time increment or load increment). At the end of each iteration of a time step, the solver evaluates the plastic strain. If the plastic strain is too high, that is, the plastic increment is greater than the value you set for Maximum Equivalent Plastic Strain Increment (PLLIM), the solver bisects the time step and restarts with a smaller time step.For more information, see Plastic strain increment limit in Plasticity analysis.
Ignore Plasticity for Pressure Sign Change (PLSHUT)	Applies when Switch off Plasticity Computation (PLSHSOL) is set to Yes at the solution level. For more information, see Nonlinear Control Parameters - Global dialog box (Simcenter Nastran).Specifies whether to ignore the plasticity computation. When Switch off Plasticity Computation (PLSHSOL) is set to Yes at the solution level:To turn off plasticity when the hydrostatic pressure sign changes, select Yes.To retain plasticity even when the hydrostatic pressure sign changes, select No.You can specify whether to ignore the plasticity at a Gauss point for the following types of subcases:Subcase - Nonlinear StaticsSubcase - Nonlinear DynamicsSubcase - Preload

Time Step Control

Automatic Timing Scheme (AUTOTIM)	Controls whether the software uses the automatic timing scheme.
Initial Time Step for Adaptive (DTINIT)	Specifies the size of the initial time step. Specify a real value that is ≥0.0.
**Maximum Time Step (DTMAX)**Minimum Time Step (DTMIN)	Specifies the minimum and maximum time step size values.For Maximum Time Step (DTMAX), specify a real value that is ≥0.0.For Minimum Time Step (DTMIN), specify a real value that is ≥0.0 and ≤ the Maximum Time Step (DTMAX) value.
Initial Time Step in a New Subcase (DTSBCDT)	Controls whether the software uses the Initial Time Step for Adaptive (DTINIT) value in a new step, or whether the software uses the time step calculated at the end of the previous step.
**Minimum Time Step Factor for Equilibrium Iteration Criterion (EQMFMIN)**Maximum Time Step Factor for Equilibrium Iteration Criterion (EQMFMX)	Specifies the minimum and maximum time step factor for the equilibrium iteration criterion. Specify a real value >0.0.
Criteria Selection (TSCCR)	Specifies the time stepping method to use.To use constant time stepping, select (0) None.To use adaptive time stepping based only on the error truncation method, select (1) Truncation Error.To use adaptive time stepping based only on the ratio of the maximum creep increment to the elastic strain method, select (2) Creep Increment to Elastic Strain Ratio.To use adaptive time stepping based on both the error truncation method and the ratio f maximum creep increment to elastic strain, select Combination of (1) and (2).To use adaptive time stepping based on both the ratio of the maximum creep increment to the elastic strain and the maximum creep increment, select Combination of (1) and (3).To use adaptive time stepping based on both the ration of the maximum creep increment to the elastic strain and the maximum creep increment, select Combination of (2) and (3).To use adaptive time stepping on the error truncation method, the ratio of the maximum creep increment to the elastic strain, and the maximum creep increment, select Combination of (1), (2) and (3).
Stepping Based on Equilibrium Iterations (TSCEQ)	Controls whether the time stepping is based on equilibrium iterations.
Stepping Based on UMAT Supplied Time Increments (TSCUMAT)	Controls whether the time stepping is based on time increments from UMAT materials.
**Minimum Time Step for UMAT Stepping (UMFMIN)**Maximum Time Step for UMAT Stepping (UMFMX)	Specifies the minimum and maximum time stepping factors for UMAT stepping.

Time Integration

Integration Scheme (TINTMTH)	Lets you specify the integration scheme to use.
Newmark Scheme Parameter 1 (BETA)	Lets you specify the first Newmark scheme parameter.
Newmark Scheme Parameter 2 (GAMA)	Lets you specify the second Newmark scheme parameter.
Hilber-Hughes Taylor Parameter (ALFA)	Lets you specify the Hilber-Hughes Taylor parameter.
Generalized-Alpha Scheme Parameter (TETA)	Lets you specify the generalized alpha methods parameter.
Modified Chung-Hulbert Scheme Parameter (RHOINF)	Defines the spectral radius at infinity.

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Nonlinear Control Parameters dialog box (Simcenter Nastran SOL 401/Simcenter 3D Multiphysics), 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 } });