Thermal-Structural Coupled Solution Parameters dialog box (Multiphysics)

Modeling Object
Name	Sets the name for the modeling object.
Label	Sets a unique numeric identifier for the modeling object.
Description	Lets you enter a description for the modeling object.
Coupling Control
Coupling Time Option	Controls the time step increment at which the software exchanges data between the solvers, up to the solution step End Time. The Simcenter Nastran solver and the Simcenter 3D Thermal solver exchange data at coupling times. The End Time is always a coupling time. Thermal Time StepThe coupling times are at each of the thermal solver time steps.Structural Time StepThe coupling times are at each of the structural solver time steps.Smaller Time Step of Coupled SolversThe coupling times are at the smallest time step increment of the two solvers within the current solution step.Solution Step End TimeThe coupling time is only at the solution step End Time.User-Specified Time StepThe coupling times are at the time step increment that you enter in User-Specified Time Step box.Note: There may be many additional coupling times, depending on any automatic time step adjustments in the solver.
Mode	Specifies the coupling mode between the Simcenter Nastran and Thermal solvers.SequentialThe structural and thermal solvers pass information to each other once per coupling time and do not attempt to converge. The starting solver solves the solution until convergence is obtained, and then the next solver solves the other solution using the values from the first solution.IterativeThe structural and thermal solvers pass information to each other for several iterations, until the variables that are being passed converge.Coupled convergence occurs when both temperatures and displacements have converged. The convergence of the coupled solution is determined by the values that you specify in the Iteration Limit, Convergence Criterion, Convergence Norm, and Relaxation options.With both modes, the thermal solver is the starting solver.
Iteration Limit	Available when Mode is set to Iterative.Sets the maximum number of coupled solve iterations for the coupled analysis if the convergence is not achieved.
Structural Convergence Control
Available when Mode is set to Iterative.
Convergence Criterion	Sets the coupled convergence value. This value must be a positive number greater than 0, but less than 1.For each iteration, convergence is checked at the solver level and then at the Multiphysics level. The structural and thermal solvers check convergence individually during their solves according to the convergence criteria that you specify:For Simcenter Nastran, you specify convergence criteria in the Nonlinear Control Parameters modeling object.For Thermal, you specify convergence criteria in the Thermal Solution Parameters modeling object.The solvers report their convergence status to Multiphysics at the end of each solve that they perform.Multiphysics monitors the coupled convergence according to the Convergence Criterion and Convergence Norm values.Multiphysics advances to the next time step when one of the following happens:The coupled Convergence Criterion is reached. The software calculates convergence by creating a ratio (according to your selected Convergence Norm) that compares the values of nodal displacements, gap distances, and contact pressures for the current step to the values at the previous step. When this ratio becomes small enough (less than your specified Convergence Criterion), the step is considered converged.The Iteration Limit (maximum number of coupled solve iterations per time step) is reached.
Convergence Norm	Specifies the type of coupling norm that is used to calculate the convergence ratio for nodal displacements, gap distances, and contact pressures.MAXUses the maximum norm convergence criterion,
Relaxation	Lets you apply a relaxation factor to the solution variables (displacements, gap distances, and contact pressures) to limit the amount these variables can change from one step to the next. A smaller value applies more relaxation to the solution variables.When the structural and thermal solutions are strongly coupled, the data being passed between the solutions can change significantly from one solution step to the next. When the variables take such large steps, the coupling convergence can be difficult. The relaxation factor can help convergence by limiting the amount these variables can change from one step to the next. The coupled solution with a relaxation factor may take longer to complete, but it may be required for a successful convergence. The resulting converged solution is generally the same with or without a relaxation factor.The relaxation factor f is applied as follows:vtarget(i)=f∙vsource(i) + (1–f) ∙ *vtarget(i-1)*where:vtarget(i) is the solution variable applied to the target solver at iteration i.vsource(i) is the solution variable computed from the source solver at iteration i.
Thermal Convergence Control
Available when Mode is set to Iterative.
Convergence Criterion	Sets the coupling convergence value for temperatures and temperature gradients through shells. This value must be a positive number greater than 0, but less than 1. For more information, see the previous discussion under Structural Convergence Control.
Convergence Norm	Specifies the type of coupling norm that is used to calculate the convergence residuals for temperatures and temperature gradients through shells.MAXUses the maximum norm convergence criterion,
Relaxation	Lets you apply a relaxation factor to the temperatures to limit the amount these variables can change from one step to the next.See the description for this option under Structural Convergence Control.
Additional Parameters
At each coupling time, temperatures on nodes and elements computed by the thermal solver are passed to the structural solver. You can specify that additional types of data are passed at each coupling time.
Pass Thermal Boundary Condition Pressures to Structural Solver	Passes pressures from Thermal Stream, Thermal Void, and Thermal Convecting Zone boundary conditions from the thermal solver to Simcenter Nastran. The software maps pressures from 1D or 2D elements computed by the thermal solver to pressures on faces and edges for the structural solver. For more information on pressure support by Simcenter Nastran, see Nodal pressure loads (Nastran and ANSYS).
Pass Structural Contact Solution to Thermal Solver	Passes contact gap distances and contact pressures on nodes from Simcenter Nastran to Thermal. Thermal computes gap thermal conductances from gap distances and pressure thermal conductances from contact pressures. The thermal solver uses gap thermal conductances when there is a gap between solid faces, and it uses the pressure thermal conductances when there is a contact. During a simulation, if the structural displacements are such that the faces switch between being separate and being in contact, then Thermal switches between using the gap thermal conductances and using the pressure thermal conductances.Sliding displacements trigger recalculation of the thermal conductances between the faces.You can use contact pressures and gap distances in expressions.
Pass Structural Displacements to Thermal Solver	Passes displacements on nodes from Simcenter Nastran to Thermal.

Learn more

Simcenter 3D Multiphysics workflow: thermal-flow-structural analysis

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Thermal-Structural Coupled Solution Parameters dialog box (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 } });