Nonlinear Control Parameters - Subcase dialog box (Simcenter Nastran SOLs 402 and 414,129)

Use this dialog box to set values for a Nonlinear Control Parameters - Subcase modeling object for SOL 402 Multi-Step Nonlinear Kinematics and SOL 414,129 Transient Response.

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 NLCNTL2 bulk entry, click Add .

To remove a parameter from the NLCNTL2 bulk entry, click Remove .

Specified Properties

The nonlinear control parameters that you added to the subcase appear here. When you add a parameter, it appears in this group the next time you edit the subcase.

Analysis Control page

Option	Description
Maximum Displacement (DISLIM)	Sets the maximum displacement that the solver can use when it predicts large displacements. When the solver reaches this value, the solve is stopped.The default value is equal to infinity.For more information, see the DISLIM parameter of the Simcenter Nastran NLCNTL2 bulk entry and the Simcenter Samcef .SUB command.Also see Stop criteria in the Simcenter Samcef solver documentation and Nonlinear effects in the Simcenter Nastran documentation.
Maximum Rotation (ROTLIM)	Sets a rotational stop value. When the solver reaches this value, the solution ends. This is useful, for example, when large displacement effects are turned off (Large Displacements (LGDISP) check box is cleared on the Solution dialog box, Parameters page), and you want to limit the solution to small displacements and rotations.When large displacement effects are turned off, the default value is 0.1. When large displacement effects are on, the default is infinity.For more information, see the ROTLIM parameter of the Simcenter Nastran NLCNTL2 bulk entry and the Simcenter Samcef .SUB command.Also see Stop criteria and Nonlinear effects in the Simcenter Nastran documentation.
Maximum Deformation (DEFLIM)	Sets the maximum strain deformation that the solver can use when it predicts large deformations (stop criteria). When the solver reaches this value, the solve is stopped.The default value is equal to the infinity unless the Large Displacements (LGDISP) check box is cleared (Solution dialog box, Parameters page). When this check box is cleared, the default is equal to 0.1.For more information, see the DEFLIM parameter of the Simcenter Samcef .SUB command.Also see in the Simcenter Samcef solver documentation and Nonlinear effects in the Simcenter Nastran documentation.
Maximum Allowed Displacement Variation (MADI)	Sets the value to limit the variation of displacements during an iteration.When the stiffness matrix is nearly singular, the variation of displacements during the iteration can be large and create numerical problems in the contact area.To minimize this variation, you can define the Maximum Allowed Displacement Variation (MADI) displacements to limit the value. If this value is negative, the maximum variation in displacement is not included in the solve. If this value is zero, the maximum value is equal to the size of the structure multiplied by 0.05. A recommended value is one-fourth to one-third of the element size in the area of contact.When you enable this option, a scaling factor of displacement (DSCAL) is displayed for each solution point in the .f06 file, in the NEWTON ITERATIONS table. You can use this information to study the effect of the MADI parameter value on resolving numerical difficulties when the stiffness matrix is nearly singular.For more information, see the MADI parameter of the Simcenter Nastran NLCNTL2 bulk entry and the Simcenter Samcef .SUB command. Also see Stiffness stabilization in the Simcenter Samcef solver documentation.
Time Unassigned Load Ramping (LVAR)	Specifies whether time-unassigned loads are ramped or stepped for this subcase. The ramping helps convergence by reducing the load increments.RampedIncrements the load starting with the value of the last load of the previous subcase to the value specified for the load in the current subcase. The solver determines the increments using the total number of time increments defined for that subcase. If a load is not specified in the previous subcase, the solver ramps from zero to the value specified for the current subcase.If your solution fails to converge, ramping the load from zero to a full load can help you to determine the load level at which the solver cannot converge. You can then examine the results at that point to try to identify the problem area in the model. SteppedSets the load directly to the specified value. The load is applied as a constant.For more information on load ramping, see Mechanical loads (SOL 401).
Time Unassigned Temperature Loads Control (TVAR)	Specifies whether time unassigned temperature loads are ramped or stepped for this subcase.RampedIncrements the temperature starting with the last temperature of the previous subcase to the temperature specified for the current subcase. The solver determines the increments using the total number of time increments defined for that subcase.If a temperature is not specified in the previous subcase, the solver ramps from zero to the temperature specified for the current subcase.SteppedSets the temperature directly to the specified value. The temperature is applied as a constant.For more information on load ramping, see Mechanical loads (SOL 401).
Displacement Prediction Using Velocities of Previous Time Step (DIPR)	Specifies whether to predict structural displacements for a time step based on the velocities of the previous time step, except for the first time step of a subcase. Select Yes to activate this prediction.In a static analysis, this prediction depends on the size of the time steps and the difference of displacements during the previous time step. This strategy is useful when the load and the derivative of the load are continuous during a subcase. The default value varies from subcase to subcase. Subcases without time-assigned loads are set to Yes, and the others are set to No. In general, follow these guidelines:If your subcases contain smooth time-assigned loads without discontinuities, select Yes.If your subcases have discontinuities, select No. Otherwise, the prediction might increase the number of iterations on those time steps.For more information, see the DIPR parameter of the Simcenter Nastran NLCNTL2 bulk entry and the Simcenter Samcef .SUB command.
Compute Norm of Internal or External Forces (NORM)	Specifies when to calculate the norm of the internal forces. This norm is used by the force error criterion that determines the convergence criteria. Calculation After AssemblyComputes the norm of the internal forces after the assembly of the forces.This default option is suitable for most situations when external loads (nodal forces, pressure, and so on) are applied to your model.Calculation Before AssemblyComputes a reference value of the norm of the internal forces before the assembly of the forces.For example, if your model has only thermal loads, the sum of internal forces may be zero (equilibrium) and the force error criterion may not be activated while perhaps the force criterion computed on local elements may be violated. Setting the Compute Norm of Internal or External Forces (NORM) to Calculation Before Assembly can help the force error criterion to trap local violations.For more information, see the NORM parameter of the Simcenter Nastran NLCNTL2 bulk entry and the Simcenter Samcef .SUB command.
Unsymmetrical Stiffness, Damping and Mass Matrices for Complex Modes (MATSYM)	Unsymmetrical matrices and the unsymmetric solver are always used for a complex modes subcase. This option is set by default for complex modes subcases and has no effect on any other subcase. For more information, see the MATSYM parameter of the Simcenter Nastran NLCNTL2 bulk entry and the Simcenter Samcef .ALG command.
Stabilization Factor (STAB)	Adds an artificial stiffness to prevent rigid bodies. This is useful when you are relying on a contact condition to prevent rigid bodies, but the contact condition is inactive at the start of the solution.The value must be small enough to avoid changing the stiffness, but not too small to avoid numerical problems.A value of 10-8 or 10-9 is recommended. In this case, the stiffness matrix is no longer singular (but it is nearly singular).For more information, see the STAB parameter of the Simcenter Nastran NLCNTL2 bulk entry and the Simcenter Samcef .SUB command. Also see Stiffness stabilization in the Simcenter Samcef solver documentation.
Include Inertia Effects for Nonlinear Dynamics Subcases (INERTIA)	Specifies whether to exclude inertia and damping when performing a dynamic analysis. This option has no effect for a nonlinear statics analysis.Exclude inertia when you need to accelerate a component and you don't want to account for vibrations. For example, you might exclude inertia in a nonlinear dynamics subcase when accelerating a tire to reach a given speed at which you want to simulate a maneuver and then include inertia for the maneuver simulation.For more information, see the INERTIA parameter of the Simcenter Nastran NLCNTL2 bulk entry.
Remove Output Results at Beginning of Non-Dependent Subcases (IAR0)	Specifies whether data is saved at the beginning of the computation of a sequentially dependent (SD) subcase.OffOmits the data from the .op2 file.OnWrites the data to the .op2 file.To make a subcase sequentially dependent, set the Sequential Dependency on Previous Subcase option on the Solution Step dialog box.For more information, see the IAR0 parameter of the Simcenter Nastran NLCNTL2 bulk entry.

Plasticity and Creep Control page

Option	Description
Creep Effects (CREEP)	Specifies whether to take creep effects into account for the subcase in which this modeling object is defined. For this option to take effect, make sure that you do the following:Select the Material Nonlinearity check box on the Solution dialog box, Parameters page. If this check box is selected, creep effects are enabled for all subcases unless you disable creep effects by selecting No and then applying this modeling object to a subcase.If this check box is cleared (material nonlinearities are disabled), you cannot use the Creep Effects (CREEP) option to enable creep effects in a subcase.Use the Manage Materials command to create or edit a material with isotropic behavior (corresponds to MAT1 bulk entry). In the Isotropic Material dialog box, click the Creep page, and from the list, select Temperature-Dependent Time Hardening (Norton-Bailey) Power Law (Type 301).Update the options to define the creep behavior (corresponds to CREEP bulk entry).For more information, see MAT1, MATCRP, CREEP, Nastran creep material properties, and Creep analysis.
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.For the backward Euler method (implicit), enter 1.0.For the trapezoidal rule, enter 0.5.For the forward Euler method (explicit), enter 0.For more information, see the CRINFAC parameter for the NLCNTL2 bulk entry.
Plasticity Effects (PLASTIC)	Specifies whether to take plasticity effects into account for this modeling object. For this option to take effect, make sure that you do the following:Select the Material Nonlinearity check box on the Solution dialog box, Parameters page. When this check box is selected, plasticity effects are enabled for all subcases unless you disable plasticity effects by selecting No and then applying this modeling object to a subcase.If this check box is cleared (material nonlinearities are disabled), you cannot use the Plasticity Effects (PLASTIC) option to enable plasticity effects in a subcase.Define a material with stress-strain data.For more information, see Define a material with stress-strain data.For more information, see MATS1 and MAT1.
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 Integration page

Option	Description
Integration Scheme (TINTMTH)	Specifies the time integration scheme for dynamic subcases. When you use an integration scheme, a rapid variation in time step size can cause a discontinuity in accelerations. If your analysis includes a rapid variation in time step size, review the options for the generalized integration schemes.NewmarkDirect time integration, one-step method, or implicit method that uses the Newton-Raphson method.Hilber-Hughes-TaylorIncludes numerical damping in the high frequency spectrum, which has a stabilizing effect on the time integration procedure while guaranteeing very good accuracy of integration of the low frequency range (including rigid body motion in particular).Generalized Midpoint MethodEnforces exact equilibrium at every time step, which guarantees second-order accuracy for damping and accelerations. This method is also less sensitive to variable time steps.Generalized AlphaEnforces equilibrium at every time step, which guarantees second-order accuracy for accelerations and less sensitivity to variable time steps.For more information, see the TINTMTH parameter for the NLCNTL2 bulk entry.
Newmark Scheme Parameter 1 (BETA)	Sets the first parameter of Newmark's method. This value is used when you set Integration Scheme (TINTMTH) to Newmark.For more information, see the BETA parameter of the Simcenter Samcef .SUB command.
Newmark Scheme Parameter 2 (GAMA)	Sets the second parameter of Newmark's method. This value is used when you set Integration Scheme (TINTMTH) to Newmark.For more information, see the GAMA parameter of the Simcenter Samcef .SUB command.
Hilber-Hughes-Taylor Parameter (ALFA)	Sets the damping parameter for the Hilber-Hughes-Taylor method. This value is ignored for all other time integration methods.The recommended value is from 0 to 0.333. For more information, see the ALFA parameter of the Simcenter Samcef .SUB command.
Generalized Midpoint Method and Generalized-Alpha Scheme Parameter (TETA)	Sets the damping parameter for the Generalized Midpoint or Generalized Alpha method. This value is ignored for all other time integration methods. For more information, see the TETA parameter of the Simcenter Samcef .SUB command.

Equilibrium Iteration and Convergence page

Option	Description
Line Search (ILNS)	Sets the line search method to be activated at a specific N Newton iteration: To disable line search, type 0.To base the line search method on minimizing energy, type a positive N integer.To base the line search method on minimizing residue, type a negative -N integer.At each Newton iteration, one line is printed in the .f06 file with the iteration number (ITER), the relative force residual (TESF), the relative energy error (TESE), the relative displacement error (TESQ), the total force residual (RES), the algorithm (NR for classical Newton-Raphson, NRM/LS for Newton-Raphson with line search), and the CPU time used for the iteration. In the .f06 file, look for the NEWTON ITERATIONS text entry.For more information, see NLCNTL2.
Line Search Convergence Tolerance (PRLN)	Sets the search convergence tolerance depending on the value for Line Search (ILNS).If Line Search (ILNS) is set to zero, this value has no effect.If Line Search (ILNS) is set to a positive integer, sets the precision threshold for line search convergence. By default, this value is 100 times the Relative Force Tolerance (PRCR) value.If Line Search (ILNS) is set to a negative integer, sets the minimum line search step at which the line search is stopped. By default, this value is 0.1. For more information, see the PRLN parameter of the Simcenter Samcef .SUB command.
Minimum Line Search Factor (AMIN)	Sets the minimum line search factor. If Line Search (ILNS) is set to zero, this value has no effect.If Line Search (ILNS) is set to a positive or negative integer, uses the minimum normalized line search factor.Leave this box blank if you want to use the solver default value:If Line Search (ILNS) is set to a positive integer, the default is 0.5.If Line Search (ILNS) is set to a negative integer, the default is 0.1.For more information, see the AMIN parameter of the Simcenter Samcef .SUB command.
Maximum Line Search Factor (AMAX)	Sets the maximum line search factor.If Line Search (ILNS) is set to zero, this value has no effect.If Line Search (ILNS) is set to a positive or negative integer, uses the minimum normalized line search factor.Leave this box blank if you want to use the solver default value:If Line Search (ILNS) is set to a positive integer, the default is 1/AMIN.If Line Search (ILNS) is set to a negative integer, the default is 2.0.For more information, see the AMAX parameter of the Simcenter Samcef .SUB command.
Maximum Bisections (MAXBIS)	Applies when Automatic Time Stepping Activation (AUTOTIM) is set to Automatic Time Stepping.Sets the maximum number of consecutive times a time step can be rejected. When a time step is rejected, the software reduces the time step using the value you set for Maximum Decrease Ratio for Next Time Step (EQMFMIN), and stars the time step again. If the number of rejections you set for Maximum Bisections (MAXBIS) is reached, the software restarts the time step one more time (Maximum Bisections (MAXBIS) plus one). If that time step is rejected, the solve stops.When a time step is accepted, the counter for Maximum Bisections (MAXBIS) is reset to zero.You can set the criteria for rejecting time steps using several options, such as:**Maximum Number of Iterations for an Implicit Time Step (ITMA)****Maximum Displacement (DISLIM)****Maximum Rotation (ROTLIM)****Maximum Deformation (DEFLIM)****Maximum Equivalent Plastic Strain Increment (PLLIM)**For more information, see Divergence criteria in the Simcenter Nastran Multi-Step Nonlinear User's Guide (SOL 401 and SOL 402).
Maximum Number of Iterations for an Implicit Time Step (ITMA)	Sets the maximum number of iterations for an implicit time step within a subcase.For more information, see the ITMA parameter of the Simcenter Samcef .SUB command.Also see the acceptable divergence information in Automatic time step choice, and see Convergence difficulties in the Simcenter Samcef documentation.
Relative Force Tolerance (PRCR)	Sets the precision threshold for the residual norm of an implicit iteration. This is the threshold for the relative force residual (TESF) convergence test value that is used in the Newton-Raphson scheme criteria. Adjust this option when your solution has convergence problems. For more information, see Newton-Raphson scheme and the PRCR parameter of the Simcenter Samcef .SUB command in the Simcenter Samcef documentation.Also see Convergence difficulties and Simcenter Nastran Multi-Step Nonlinear User’s Guide (SOL 401 and SOL 402).
Reference Force (REFP)	Sets the reference value for the force convergence error function. This value is the increment for the sum of the internal and external inertia forces that is used in the Relative Force Tolerance (PRCR) criterion.For more information, see the REFP parameter of NLCNTL2 and Simcenter Nastran Multi-Step Nonlinear User’s Guide (SOL 401 and SOL 402). Also see the TREF parameter of the .SUB command in the Simcenter Samcef documentation.
Relative Displacement Tolerance (PRCQ)	Sets the relative displacement tolerance for convergence. This is the threshold for the relative displacement/temperature residual (TESQ) that is used in the Newton-Raphson convergence criteria. For more information and the default value, see the PRCQ parameter of the Simcenter Nastran NLCNTL2 bulk entry. Also see Newton-Raphson scheme and the PRCQ parameter of the Simcenter Samcef .SUB command in the Simcenter Samcef documentation.For information on convergence, see Convergence difficulties and Simcenter Nastran Multi-Step Nonlinear User’s Guide (SOL 401 and SOL 402).
Reference Displacement (REFU)	Sets the reference displacement value that is used in the Relative Displacement Tolerance (PRCQ) criterion.For more information, see the REFU parameter of NLCNTL2 and Simcenter Nastran Multi-Step Nonlinear User’s Guide (SOL 401 and SOL 402). Also see the QREF parameter of the .SUB command in the Simcenter Samcef documentation.
Relative Energy Tolerance (PRCE)	Sets the relative energy tolerance. This is the threshold for the energy convergence test value (TESE) that is used in the Newton-Raphson convergence criteria.For more information, see Newton-Raphson scheme and the PRCE parameter of the Simcenter Samcef .SUB command in the Simcenter Samcef documentation.Also see Convergence difficulties in the Simcenter Samcef documentation and Simcenter Nastran Multi-Step Nonlinear User’s Guide (SOL 401 and SOL 402).
Reference Energy (REFE)	Sets the reference energy. This value is used in the energy residual criterion, Relative Energy Tolerance (PRCE).For more information, see the REFE parameter of the NLCNTL2 bulk entry, and Simcenter Nastran Multi-Step Nonlinear User’s Guide (SOL 401 and SOL 402).Also see the EREF parameter of the .SUB command in the Simcenter Samcef documentation.
Relative Contact Forces Tolerance (PRCF)	Sets the precision threshold for the variation of contact forces. The solver computes a relative contact force residual named TESC, and prints it at each iteration in the .f06 file. For your solution to converge, the TESC value must be smaller than the Relative Contact Forces Tolerance (PRCF) value. Thus, compare the value you enter for Relative Contact Forces Tolerance (PRCF) with the TESC value in the .f06 file and adjust the value for Relative Contact Forces Tolerance (PRCF) as necessary.For more information, see the PRCF parameter of the NLCNTL2 bulk entry, and see Contact convergence.
Zero-Load Convergence Option (OTRE)	Enables easier convergence when no external loads are applied, that is, for rigid body motion.DisabledUse this when the time step does not converge after four iterations but less than 10 times the convergence criteria. If that occurs, select this option to strictly enforce convergence tolerances.Ignore Force Convergence if lower than 10*PRCR for Iterations 2 to 4Marks the subcase as converged when the following are true:Both the Relative Energy Tolerance (PRCE) and Relative Displacement Tolerance (PRCQ) convergence criteria are satisfied for iterations 2 through 4.The relative force residual (TESF) convergence test value is less than 10 times the threshold value set by Relative Force Tolerance (PRCR). For example, if Relative Force Tolerance (PRCR) is set to 0.001, the relative force residual must be less than 0.01.Ignore Force Convergence + Automatic REFPUses the value for Relative Force Tolerance (PRCR) as the residual for the first iteration of the subcase, and marks the subcase as converged when it meets the criteria for Ignore Force Convergence if lower than 10*PRCR for Iterations 2 to 4.For more information, see the OTRE parameter of the NLCNTL2 bulk entry.
Stiffness Update Strategy Parameter 1 (IT1K)	In addition to the classical Newton-Raphson scheme, in which a new iteration matrix is computed at each iteration, you can define a variant of the Newton-Raphson scheme, in which the iteration matrix is updated only at specific time step iterations.To do this, you define two iteration numbers (Stiffness Update Strategy Parameter 1 (IT1K) and Stiffness Update Strategy Parameter 2 (IT2K)) and a frequency (Stiffness Update Strategy Parameter 3 (IT3K)), so that the matrix is updated at iteration numbers IT1K, IT2K, IT2K+IT3K, IT2K+2 ×IT3K, and so on.Between these iteration numbers, the matrix remains unchanged.Note: These values are iteration numbers (integers), not time values.Use Stiffness Update Strategy Parameter 1 (IT1K) to set the first iteration number that determines when the iteration matrix is updated. For more information, see the IT1K parameter of the Simcenter Samcef .SUB command.
Stiffness Update Strategy Parameter 2 (IT2K)	Sets the second iteration number that determines when the iteration matrix is updated. For more information, see the IT2K parameter of the Simcenter Samcef .SUB command.
Stiffness Update Strategy Parameter 3 (IT3K)	Sets the frequency of the iteration matrix updates. For more information, see the IT3K parameter of the Simcenter Samcef .SUB command.
Variation of Stresses for a Plastic Material (PLAS)	For plastic material, specifies the constitutive law integration scheme (tangent matrix integration and computation of the variation of stresses) at the first iteration of each time step. To help with convergence:If your structure is loaded, select Plastic Tangent Matrix, Plastic Computation or Plastic Tangent Matrix, Elastic Computation. If your structure is unloaded, select Elastic Tangent Matrix, Plastic Computation or Elastic Tangent Matrix, Elastic Computation. If your structure has thermal loads, select Elastic Tangent Matrix, Elastic Computation or Plastic Tangent Matrix, Elastic Computation.For more information, see the PLAS parameter of the Simcenter Samcef .SUB command.
Thermal Loads Management (ITHE)	Specifies how to compute the equilibrium between external forces and temperatures when the analysis includes temperature loads. The optimal selection depends on how the structure to which the temperature loads are applied is constrained. The results for both options are the same. The difference is in how quickly the solution converges.Constrained Thermal Expansion (Default)Adjusts how mechanical strain is computed to account for temperature loads on a model that is fully constrained. If the structure is fully constrained and cannot expand freely, select this option.For example, if temperature loads are applied to a beam that is constrained at both ends, the structure cannot expand freely. This can cause forces and stresses in the beam, high thermal stresses and strains, possibly solution instability, and long solving times. Selecting Constrained Thermal Expansion adjusts how temperature is handled in each time step to lead to quicker convergence.Free Thermal ExpansionAdjusts how mechanical strain is computed to account for temperature loads on a model that is free to expand. If the structure is partially constrained and can expand, select this option. For example, if temperature loads are applied to a beam that is constrained at only one end, the beam can expand freely in response to the temperature loads. Other examples of structures that are typically free to expand include blades and turbomachinery.For more information, see the ITHE parameter of NLCNTL2.

Automatic Time Stepping page

Automatic time stepping is recommended for nonlinear dynamic subcases.

Option	Description
Automatic Time Stepping Activation (AUTOTIM)	Specifies whether you want fixed or automatic time steps.For more information, see the AUTOTIM parameter of the NLCNTL2 bulk entry.
Size of First Step (DTINIT)	Sets the length of the first time step. To let the solver compute the size of the first time step, leave this box blank. The size of each time step is determined by convergence criteria and the integration error of differential equations.For more information, see the DTINIT parameter of the NLCNTL2 bulk entry.
The following options apply when Automatic Time Stepping Activation (AUTOTIM) is set to Automatic Time Stepping.
Minimum Time Step (DTMIN)	Sets the minimum time step size for all time steps. If the time step becomes smaller than this value, the computation is stopped. To let the solver use the DTINIT default value, leave this box blank.For more information, see the DTMIN parameter of the NLCNTL2 bulk entry.
Maximum Time Step (DTMAX)	Sets the maximum time of a time step. To let the solver use the infinite default value, leave this box blank.Note: Depending on the prescribed list of times, to reach the next prescribed time, the solver might choose a time step value that is slightly larger than the DTMAX value to avoid using a succession of large time steps that are followed by a single tiny time step. For example, if the next prescribed time step is in (10+ε)*DTMAX, the solver might perform 10 time steps of (1+ε/10)*DTMAX.For more information, see the DTMAX parameter of the NLCNTL2 bulk entry.
Maximum Increase Ratio for Next Time Step (EQMFMX)	Sets the maximum factor the solver can use to increase the current time step value for the next time step. This value is unitless. For more information, see the EQMFMX parameter of the NLCNTL2 bulk entry.
Maximum Decrease Ratio for Next Time Step (EQMFMIN)	Sets the maximum factor the solver can use to reduce the current time step value for the next time step. This value is unitless. For more information, see the EQMFMIN parameter of the NLCNTL2 bulk entry.
Activation of Time Step Criterion Using PRED (ERCD)	Specifies whether to activate the time step acceptance criterion based on the absolute error of the change in displacement. For more information, see the ERCD parameter of the Simcenter Nastran NLCNTL2 bulk entry, and of the Simcenter Samcef .SUB command. Also see Automatic time step choice in the Simcenter Samcef solver documentation.
Absolute Allowable Displacement Change (PRED)	Sets the maximum allowable displacement in one time step for the time step criterion. If the limit is reached, the time step is rejected, and the solution is stopped with an error. For more information, see the PRED parameter of the Simcenter Nastran NLCNTL2 bulk entry, and of the Simcenter Samcef .SUB command. Also see Stiffness stabilization in the Simcenter Samcef solver documentation.
Optimal Number of Iterations (ITEREF)	Sets the number of iterations used by the automatic time stepping scheme. The default is 0.6 times the Maximum Number of Iterations for an Implicit Time Step (ITMA) option on the Equilibrium Iteration and Convergence page.If the solver needs more iterations to converge, it continues the solve, but with a smaller time step. On the other hand, if the solver needs fewer iterations to converge, it increases the time step.For more information, see the ITEREF parameter of the NLCNTL2 bulk entry.
Integration Error Control (TSDYN)	Specifies whether you want error control. For a dynamic analysis, the software computes an estimate of the error made during the integration of the differential equation. If Integration Error Control (TSDYN) is set to On, the time step is rejected if the error is larger than the value set for Integration Error Control Threshold (PRCO), unless the time step is smaller than the limit set by Time Step Limit for Integration Error (HPRCO).For more information, see the TSDYN parameter of the NLCNTL2 bulk entry.
Time Step Limit for Integration Error (HPRCO)	Sets the time value for the integration error control parameter. This value is used when you set both of the following:Integration Scheme (IMPL) to Hilber-Hughes-Taylor or Newmark.Integration Error Control (TSDYN) to On.The integration error is not checked if the time step value is smaller than this value.For more information, see the HPRCO parameter of the Simcenter Nastran NLCNTL2 bulk entry, and of the Simcenter Samcef .SUB command.
Integration Error Control Threshold (PRCO)	Sets the precision threshold for the integration error of the dynamic equation.For more information, see the PRCO parameter of the Simcenter Nastran NLCNTL2 bulk entry, and of the Simcenter Samcef .SUB command.
Zero Pivot Time Step Rejection (RJPZ)	Specifies whether you want to reject time steps when zero pivots are detected. Often zero pivots appear during the first time step if the model has rigid body modes.For more information, see the RJPZ parameter of the NLCNTL2 bulk entry.
Negative Pivot Time Step Rejection (RJPN)	Specifies how you want the solver to handle time steps when negative pivots are detected. In nonlinear analyses, negative pivots are a negative stiffness that appear when critical loads (instabilities) are overshot or when Newton method diverges strongly. Often negative pivots occur when the loading becomes too high.NeverNever but Print at Last IterationIf Last Iteration****AlwaysFor more information, see the RJPN parameter of the NLCNTL2 bulk entry.
Viscous Material Integration Error Control (TSCVSC)	Activates time step criterion based on material integration.Note: The viscous material integration options are advanced options for specialized materials. For most analyses, you can omit these options.For more information, see the TSCVSC parameter of the Simcenter Nastran NLCNTL2 bulk entry or the VISC parameter of the Simcenter Samcef .SUB command.
Viscous Material Integration Error Threshold (VSCOTE)	Sets the precision threshold for the integration error of the viscous material. The time step is adjusted to keep the local error under this limit. Local error is the error computed for each Gauss point divided by the Viscous Material Minimum Stress Normalization Factor (VSCOSN). For the local error calculation, see Time step in Basic Viscoelastic Behaviors or Visco-plastic Behavior.This value is used when Viscous Material Integration Error Control (TSCVSC) is set to On.For more information, see the VSCOTE parameter of the Simcenter Nastran NLCNTL2 bulk entry or the PRCV parameter of the Simcenter Samcef .SUB command.
Viscous Material Minimum Stress Normalization Factor (VSCOSN)	Sets the reference stress of the material. The value you use depends on the material load, and it is used in the calculation to determine the local error. To see how this reference value is used in the calculation, see Time step in Basic Viscoelastic Behaviors or Visco-plastic Behavior.This value is used when Viscous Material Integration Error Control (TSCVSC) is set to On.For more information, see the TSCVSC parameter of the Simcenter Nastran NLCNTL2 bulk entry or the SREF parameter of the Simcenter Samcef .SUB command.

Restart Options page

Option

Description

Restart Computation Flag (RSUB)

Sets the subcase number that you want to use for an internal restart. The solver fetches the final computation state (displacements, velocities, stresses, state variables, and so on) from this subcase to apply to the beginning of the current subcase. This is useful, for example, when you want to apply a preload computation for bolts to several subcases without recomputing the preload. Note: If your solution has time-dependent loads and sequentially dependent subcases, you must ensure a smooth transition to the subcase that uses the previous subcase's computation state. For example, if your solution has four subcases, and you want subcase 4 to restart from subcase 2, you must ensure that the boundary conditions between the end of subcase 2 and the beginning of subcase 4 are consistent. If the boundary conditions are not consistent, the loads can become discontinuous, which can cause potential shocks, vibrations, and nonconvergence issues. A sequentially dependent (SD) subcase also uses the final time of the previous subcase for its start time. The computation state (stresses, strains, and so on) when the SD subcase starts is the state of the final time of the previous subcase. However, a non-sequentially dependent (NSD) subcase uses the final time of the previous subcase for its start time, and its starting state can be determined by the Restart Computation Flag (RSUB) parameter:-1The computation state (stresses, strains, and so on) when the NSD subcase starts is the state of the final time of the previous subcase, as for a SD subcase.0The computation state (stresses, strains, and so on) when the NSD subcase starts is reset so that the state is the same as at the initial time of the solve. The solver does not use a state from any previous subcase computation unless you request an initial static computation. N>0The computation state (stresses, strains, and so on) when the NSD subcase starts is the state of the final time of the previous subcase N.Note: Subcases always restart from the final time (except when RSUB=0) of the preceding or assigned subcase. You cannot restart at a computation time inside of a subcase interval.For more information, see Internal restarts (SOL 402).

Contact Options page

Note:

The default values for the contact parameters are optimized for most solutions. We recommend that you attempt to solve the solution before you change these values.

Option	Description
Relaxation Factor for Contact (RELC)	Sets the relaxation factor for contact degrees of freedom. The relaxation factor is used in determining the number of iterations to solve a contact. At each iteration, the contact degrees of freedom is multiplied by this number. The relaxation iterations are performed as long as the convergence criterion is greater than the threshold. This relaxation factor works only on the Lagrange multipliers. You can use it to facilitate the convergence of the Newton-Raphson procedure in the presence of contacts, but that may lead to more iterations.This relaxation is performed as long as the convergence criterion (TESF) is greater than the threshold. The threshold value is equal to 10 times Relative Force Tolerance (PRCR).Relaxation Factor for Contact (RELC) values less than 1.0 result in under-relaxation. Values greater than 1.0 result in over-relaxation and a value equal to 1 matches the pure Newton-Raphson method. A characteristic value for relaxation coefficient is 0.7. For more information, see the RELC parameter of the Simcenter Samcef .SUB command. Also see Convergence difficulties.
Characteristic Length for Contact (DCON)	Sets the inactive distance (between the slave node and the target surface) above which no contact occurs. To let the solver compute the characteristic length based on element sizes, leave this box blank.For more information, see the DCON parameter of the Simcenter Samcef .SUB command.
Regularization Factor for the Augmented Lagrange Multipliers (PRCS)	Sets the regularization factor for the augmented Lagrange multipliers.To let the solver compute the regularization factor from the average stiffness of the whole model, leave this box blank.For more information, see the PRCS parameter of the Simcenter Samcef .SUB command.
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 must define the Tangential Contact Stiffness in Linear Perturbation Subcase (KMODTN) in a Nonlinear Control Parameters - Subcase modeling object at the solution level. You can vary other Nonlinear Control Parameters - Subcase parameters from subcase to subcase.For more information, see the KMODTN parameter of the Simcenter Nastran NLCNTL2 bulk entry.

Diagnostic Listing File Printout page

Option	Description
Printing Frequency of General Results (IMPG)	Sets the printing frequency of general information such as number of contacts, number of plastic elements, and so on. To print this information in the .f06 file at every time step, enter 1. Otherwise, enter 2 to print at every other time step, enter 3 to print at every third time step, and so on.For more information, see the IMPG parameter of the Simcenter Samcef .SUB command.
Hit-Parade of Residuals to be Printed in Listing File (IMPR)	Sets the number of the maximal residuals to be printed in the .f06 file. For example, to print the 10 largest residuals, enter 10.Reviewing a list of the largest residuals can help you to isolate problem areas, such as a node that occurs in each residual.For more information, see the IMPR parameter of the Simcenter Samcef .SUB command. Also see Convergence difficulties and Contact modeling.
Maximum Number of Pivots Printed in Listing File (IMPV)	Sets the maximum number of pivots (negative or zero) to print in the .f06 file.In nonlinear mechanics, negative pivots represent a negative stiffness that appears when critical loads (instabilities) are overshot or when the Newton method diverges strongly. Negative pivots appear when the loading becomes too high. Zero pivots can be degrees of freedom without any stiffness, redundancy of constraints and/or boundary conditions, and rigid body modes. The solver fixes these zero pivots and relaxes them if the pivot disappears (unless they were discovered at the very beginning of the computation).For more information, see the IMPV parameter of the Simcenter Samcef .SUB command.

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

SOL 402 nonlinear capabilities

Nonlinear Control Parameters - Subcase dialog box (Simcenter Nastran SOLs 402 and 414,129), 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 } });