Multiphysics

Defining multiphysics solution steps

Simcenter 3D Multiphysics solution steps are equivalent to subcases in Simcenter Nastran. Solutions in the Simcenter 3D Thermal/Flow solver environment have no notion of steps.

Starting solver and initial conditions

The thermal, flow, or thermal-flow solver always starts the coupled solution.

The first solution step determines the initial condition for the thermal, flow, or thermal-flow solver, and can be the result of a thermal/flow solve or your predefined initial temperature, depending on the selected thermal/flow solution type.

If the first solution step is transient, no thermal/flow solve is performed, and the global initial conditions are passed to the structural solver.
If the first solution step is steady-state, a steady-state thermal/flow solve determines the initial conditions.

Sequence of steps and sequential dependency

The sequence of solution steps is based on the End Time that you define for each solution step on the Time Step Definition page.

By default, a solution step is sequentially dependent on the results of the previous solution step. That is, the current solution step receives the final state variables (such as displacements) from the previous solution step. The current solution step’s start time is the End Time of the previous solution step.

You can disable this dependency by setting Sequential Dependency on Previous Subcase on the Step Control page to No. When this option is set to No, the start time of the solution step is 0.

In the Structural Control group and Thermal Control, Flow Control, or Thermal Flow Control groups, choose the appropriate Time Step Option to specify how the structural solver and thermal, flow, or thermal-flow solver subdivide a solution step into time steps. For more information, see Controlling time steps in a coupled solution.

Solution step types

You can define a solution step as one of these types:

Thermal, Flow, and Thermal Flow

Steps that are created when Analysis Type is set to Thermal, Flow, or Coupled Thermal-Flow, respectively. In these thermal/flow steps, you specify the solution type, time step definition, and results options.

The thermal/flow solution can be steady state or transient. If you define a transient solution step, you must have at least two transient steps in the solution.

The flow solver does not support a mix of steady-state and transient solution steps in the same solution.

Nonlinear Statics

A static solution in which loads can be constant or time assigned.

This type of solution step can include geometric and material (plasticity or creep) nonlinearity.

Nonlinear Dynamics

A dynamic solution in which loads can be constant or time assigned.

This type of solution step can include geometric and material (plasticity or creep) nonlinearity.

Thermal Nonlinear Statics, Flow Nonlinear Statics, and Thermal Flow Nonlinear Statics

Coupled step in which the structural solver exchanges data through the Multiphysics application with the thermal, flow, or thermal-flow solver, respectively.

These steps combine information from thermal/flow steps with information from Nonlinear Statics structural step.

Thermal Nonlinear Dynamics, Flow Nonlinear Dynamics, and Thermal Flow Nonlinear Dynamics

Coupled step in which the structural solver exchanges data through the Multiphysics application with the thermal, flow, or thermal-flow solver, respectively.

These steps combine information from thermal/flow steps with information from Nonlinear Dynamics structural step.

Normal Modes

Specialized structural step that runs a modal analysis. This step can include stress stiffening, follower stiffness, and the spin softening from the previous thermal nonlinear static solution step.

Preload

Specialized structural step for a Bolt Pre-Load (including contact and glue) or Temperature load. Preload steps must have an End Time of 0. Any solution step that precedes a Preload step must also have an End Time of 0. You can have only one Preload step in a solution.

The thermal solver performs a steady-state calculation in the pre-load step for a coupled solution.

Cyclic Modes

Cyclic symmetric step that supports the cyclic symmetric solution for normal modes at higher harmonic indices. The software computes the modes about the nonlinear stress or displacement state at the end of a previous static step in the solution. It allows you to specify the harmonics for which to solve or choose a set of harmonics you define using the Harmonics Set modeling object.

Output of solution data

During the course of a coupled analysis, the structural, thermal, and flow solvers perform many solves. You may want to output data for post processing at each of these solution points or only at certain points. You can control this output using the Output Flag option, which is located in the Time Step Definition page, under the Output Control group. You can specify that the software should output data at the following times.

Requested Increments

Outputs data at each of the time step increments for the structural, thermal, and flow solvers.

Solution Step End Time

Outputs data only at the End Time for the solution step.

All Coupling Times

Outputs data only at the coupling times, which, depending on the Coupling Time Option, may be the same as requested increments.

All Times

Outputs data:

At all structural time steps and all coupling times for structural analysis.
At all thermal time steps and all coupling times for thermal analysis.

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

Controlling time steps in a coupled solution

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