Nonlinear Control Parameters - Global dialog box (Simcenter 3D Multiphysics)

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.

Global Parameters tab

Option	Description
Allow Chocking Behavior (CHOCK)	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. When Switch off Plasticity Computation (PLSHSOL) is set to Yes, you must also turn off the plastic computation at the subcase level by setting 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.

Advanced Parameters tab

Option	Description
Stress-Strain Conversion Method (STRCONV)	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 modulus	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

Restart Parameters tab

Appears when Structural or Coupled Thermal-Structural is selected as the analysis type.

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 tab 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 tab override over those on the Restart Management page.

Option	Description
Generate Restart Point (RSTGEN)	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. The data is saved in the .op2 file.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, and it cannot precede the subcase you set in Subcase ID of Initial Run to Restart from (RSTFROM).
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 tab

The Obsolete Parameters tab 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

Output Label for Element Stress-Strain Measures (STROUT)

This parameter is no longer supported as of the Simcenter Nastran 2020.2 release. 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). 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.*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).

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 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 } });