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

Step	Summary	Detailed help topic
1.	Create a FEM and mesh the model.	Create a FEM using the Simcenter 3D Multiphysics FEM template. Set Solver to Simcenter 3D Multiphysics and Analysis Type to one of the following:Coupled Thermal-StructuralCoupled Flow-StructuralCoupled Thermal-Flow****Coupled Thermal-Flow-StructuralMesh the model. With these analyses, the same mesh can be used for both the structural and thermal part of the model.For each mesh collector, choose the appropriate material and physical properties for your analysis.	Create a new FEM fileMeshingPhysical properties and element attributesMaterials
2.	Create a simulation	Create a simulation using the Simcenter 3D Multiphysics Sim template.	Create a new Simulation file
3.	Create the solution	Create a new solution with Solver set to Simcenter 3D Multiphysics and Analysis Type set to the same analysis type as in FEM.Alternatively, you can create a solution directly from a predefined condition sequence, to describe a time history of conditions applied to a structure throughout the course of a mission or duty cycle.	Using a condition sequence to define a solution
4.	Specify maximum number of iterations and other control parameters	In the Solution dialog box, on the Solution Control page, create a Nonlinear Control Parameters modeling object. You can specify options such as the maximum number of iterations per time step, whether to use the element iterative solver, whether to include creep effects, and so on. These parameters correspond to the NLCNTL bulk data entry for the structural solver.	Nonlinear Control Parameters dialog box (Simcenter Nastran SOL 401/Simcenter 3D Multiphysics)
5.	Adjust thermal solution parameters	In the Solution dialog box, on the Solution Control page, create a Thermal Solution Parameters modeling object, where you can adjust the thermal and radiation parameters.	Setting thermal solver parametersUnderstanding radiation parameters
6.	Adjust flow solution parameters	In the Solution dialog box, on the Solution Control page, create a Flow Solution Parameters modeling object, where you can adjust the flow solver parameters, such as time step, convergence criteria, freeze flow parameters, and relaxation factors.	Setting flow solver parametersDefining a time step for a flow analysisUnderstanding the freeze flow field optionsSetting relaxation factors for the flow solver
7.	Adjust structural solution parameters	In the Solution dialog box, on the Solution Control page, create a Structural Solution Parameters modeling object. These parameters correspond to the PARAM bulk data entry for the structural solver.	Structural Solution Parameters dialog box (Multiphysics)
8.	Enable geometric or material nonlinear effects	In the Solution dialog box, on the Solution Control page, select Large Displacements to model geometric nonlinear effects for the solution steps.If you have creep or plasticity defined in your model, you must select Material Nonlinearity to enable it in the solution. This option corresponds to the MATNL parameter.	Geometry nonlinearity overviewMATNL
9.	Define coupled solution parameters	Specify how the solver should calculate the next time step, whether the coupling should be sequential or iterative, specify the types of data to pass between the thermal, flow, and structural solvers, and at what times that data should be passed.	Define coupled solution parametersControlling time steps in a coupled solution
10.	Specify the initial conditions for the thermal and flow solvers	On the Initial Conditions page of the Solution dialog box, specify the initial temperature for the thermal solver and initial flow conditions for the flow solver.	Thermal initial conditions3D flow initial conditions
11.	Specify the stress-free reference temperature for the structural solver	In a coupled analysis, the load temperatures come directly from the thermal/flow solver, but you must specify the stress-free reference temperature for the structural solution. To specify this reference temperature, create an Initial/Stress Free Temperature type of Temperature Set and optionally create Temperature loads.	Modeling thermal strain in a Nastran analysis
12.	Request the types of results to output	The Structural Output Request, Thermal Output Request, Flow Output Request, and Thermal-Flow Output Request modeling objects specify the types of results to recover from the solution, for example, displacements, stresses, temperatures, and flow velocity.You can specify output requests both for the solution and for individual solution steps.	Requesting structural output for Simcenter 3D MultiphysicsRequesting thermal, flow, and thermal-flow output for Simcenter 3D Multiphysics
13.	Define a preload (structural) solution step	To define a bolt preload, create a Preload type of structural solution step. This step should be placed before all static solution steps in which you plan to include the bolt preload.You can also include Temperature loads in a Preload step.	Bolt pre-loads with Simcenter Nastran and Simcenter 3D MultiphysicsDefining multiphysics solution steps
14.	Define coupled solution steps	Create one or more coupled solution steps to define thermal-flow-structural exchange of data. This step can also include geometry and material plasticity or creep nonlinearity.In each coupled solution step, you can define the thermal-flow solution type as Steady State or Transient. If you choose Transient, you must define at least two coupled solution steps.
15.	Define a normal modes (structural) solution step	Create a Normal Modes type of solution step, which can use the stiffness condition (such as stress stiffening, follower stiffness, and spin softening) from the previous static solution step.The Nonlinear Control Parameters modeling object determines whether the stiffness conditions are used:FOLLOWK — Include follower stiffness.SPINK — Include spin softening.STRESSK — Include stress stiffening.
16.	Add constraints, loads, glue, and contact	Add thermal, flow, and structural constraints and loads in the Simulation file. Loads can be static or time assigned.You can add constraints at the solution level or to individual steps. You can add loads only at the solution level. You can organize loads within load sets.	Boundary conditionsUsing fields and expressions to define boundary conditionsSimcenter 3D Multiphysics boundary conditions
17.	Add contact and glue conditions	Add glue and contact conditions to the model as needed.	Contact and glue overview (Simcenter Nastran, Simcenter 3D Multiphysics)Surface-to-Surface Contact (Simcenter Nastran, Simcenter 3D Multiphysics, Abaqus, ANSYS)Edge-to-Edge Contact (Simcenter Nastran, Simcenter 3D Multiphysics)Surface-to-surface gluing (Simcenter Nastran, Simcenter 3D Multiphysics)Edge-to-Edge Gluing (Simcenter Nastran, Simcenter 3D Multiphysics)
18.	Solve the solution	Solve the solution to generate the analysis results. The Solution Monitor displays the solve progress for the Simcenter 3D Multiphysics coupled solution, Simcenter 3D Thermal, Simcenter 3D Flow, and Simcenter Nastran.	Solve the model
19.	Analyze results	Use post processing tools, such as contour plots and XYZ graphing, to analyze your results.	Analyzing multiphysics results

Learn more

Simcenter 3D Multiphysics workflow: structural solution using one-way coupling of temperature loads

Simcenter 3D Multiphysics workflow: mapping temperatures onto a structural model

Simcenter 3D Multiphysics workflow: coupled thermal-structural analysis with an external CFD solver

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

Simcenter 3D Multiphysics workflow: thermal-flow-structural analysis, 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 } });