Controlling time steps in a coupled solution

In a Simcenter 3D Multiphysics solution step, the structural, thermal, and flow solvers perform their respective solves at each time step. This page describes how to control time steps for the following coupled analyses:

• Coupled Thermal-Structural

• Coupled Flow-Structural

• Coupled Thermal-Flow-Structural

The thermal solver, flow solver, or thermal-flow solver in these coupled analyses is always the starting solver. You can control the time steps taken by each solver separately.

The time steps for a solution step correspond to the TSTEP1 bulk data entry in Simcenter Nastran.

Note:

The thermal/flow portion of a solution step can be a transient or steady-state solution. If your solution step specifies that the thermal/flow solution type is steady-state, the thermal solver, flow solver, or thermal-flow solver does not consider time steps. Instead, it performs a steady-state solve according to the coupling time option (see Specifying coupling times below), with time evaluated at the coupling time.

The structural portion of a solution step is a static solution, and time is used only as the mechanism to increment loads.

You can control the time steps in a solution step by specifying the End Time and Number of Increments for that step. The End Time applies to both the structural and thermal/flow solver, but you can define a separate Number of Increments value for each solver.

The time steps for a solution step are determined by:

time steps = (current solution step End Time – the previous solution step End Time) / Number of Increments

Consider the following examples.

Previous solution step End Time (sec)	Current solution step End Time (sec)	Number of Increments	Time steps (sec)
0.0	10.0	1	10.0
0.0	10.0	5	2.0, 4.0, 6.0, 8.0, 10.0
15.0	20.0	2	17.5, 20.0

Note:

The solvers may modify the time step increment dynamically, depending on whether Automatic time stepping is used in the thermal solver, and whether creep is defined in the structural solver.

The flow solver does not support automatic time stepping.

You specify the Number of Increments in the Solution Step dialog box on the Time Step Definition page. The time steps for a solution step correspond to the TSTEP1 bulk data entry in Simcenter Nastran.

Note:

Alternatively, you can specify a constant Step Size in terms of time.

Specifying coupling times

The structural solver and the thermal/flow solver exchange data at coupling times. At each coupling time, temperatures on nodes and elements (from the thermal solution) are passed to the structural solver. You can specify that additional types of data are passed at each coupling time using the options in the Coupled Solution Parameters modeling objects for the solution.

You can control the time step increment at which Multiphysics exchanges data between the solvers, up to the solution step End Time. The End Time is always a coupling time. By default, the coupling times are at each of the thermal/flow solver time steps. Coupling times are added automatically as common integration time points for all solvers.

To change the coupling time basis, you can use the Coupling Time Option on the Coupled Solution Parameters dialog boxes:

Thermal Time Step (default)

The coupling times are at each of the thermal solver time steps.

Example:

Suppose the end time for the previous solution step is 0.0 and the end time for the current solution step is 10.0 seconds.

Solution step End Time (sec)	Solver	Number of Increments	Time steps (sec)
10.0	Simcenter Nastran structural	4	2.5, 5.0, 7.5, 10.0
Simcenter 3D Thermal/Flow	5	2.0, 4.0, 6.0, 8.0, 10.0

The coupling times are at 2.0, 4.0, 6.0, 8.0, and 10.0 seconds.

Note:

There may be many additional coupling times, depending on any automatic time step adjustments in the thermal solver if the flow solver is not present.

Flow Time Step

The coupling times are at each of the flow solver time steps.

In thermal-flow and thermal-flow-structural solutions, the thermal and flow solvers always have the same number of increments.

Structural Time Step

The coupling times are at each of the structural solver time steps. Using the previous example, the coupling times are at 2.5, 5.0, 7.5, 10.0 seconds.

Note:

There may be many additional coupling times, depending on any automatic time step adjustments in the solver.

Smaller Time Step of Coupled Solvers

The coupling times are at the smallest time step increment of all the solvers within the current solution step.

Using the previous example, the smaller time step is 2.0 seconds; therefore, the coupling times are at 2.0, 2.5, 4.0, 5.0, 6.0, 7.5, 8.0, and 10.0 seconds.

Note:

There may be many additional coupling times, depending on any automatic time step adjustments in the solver. If you have creep defined in the structural solution, the structural solver may create many very small time steps, and using this Coupling Time Option may adversely affect the solve performance.

Solution Step End Time

The coupling time is only at the solution step End Time.

User-Specified Time Step

The coupling times are at the time step increment that you enter.

Using sequential or iterative coupling

In the Coupled Solution Parameters for the solution, you can specify the coupling Mode option.

Sequential

The structural solver and the thermal/flow solver pass information to each other once per coupling time and do not attempt to converge together. The software solves the first solution until convergence is obtained, and then solves the other solution using the values from the first solution.

Iterative

The structural solver and the thermal solver pass information to each other for several iterations, until the variables that are being passed converge. This method requires you to specify the Iteration Limit, Convergence Criterion, Convergence Norm, and Relaxation values. Coupled convergence occurs when both temperatures and displacements have converged.

The flow solver does not support this option.

How do I

Define coupled solution parameters

Learn more

Simcenter 3D Multiphysics overview

Mapping results data to another model in Simcenter 3D Multiphysics

Two-way fluid-structure interaction

Defining multiphysics solution steps

Requesting structural output for Simcenter 3D Multiphysics

Requesting thermal, flow, and thermal-flow output for Simcenter 3D Multiphysics

Adding time points to a structural solution to match a reference solution

Previewing Multiphysics solver syntax

Analyzing multiphysics results

Controlling the export of nodes connected to flow elements

Look up more details

Simcenter 3D Multiphysics boundary conditions

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Related Topics

SOL 401 nonlinear capabilities

Controlling time steps in a coupled solution, 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 } });