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

Step	Summary	Detailed help topic
1.	Create the thermal simulation file and solution.	Create a thermal simulation file and solution using the Simcenter 3D Multiphysics Sim template. Set the Solver to Simcenter 3D Multiphysics and set the Analysis Type to Thermal.	Create a new FEM fileMeshing for Simcenter 3D Thermal/Flow, Electronic Systems Cooling, Space Systems ThermalPhysical properties and element attributesDefining materials for Simcenter 3D Thermal/Flow, Electronic Systems Cooling, and Space Systems ThermalSolution dialog box (Multiphysics)
2.	Solve the thermal model.	Solve the thermal solution to output the .bun file that contains the temperature results.
3.	Open or create the structural model.	Create the structural FEM and simulation file using the Simcenter 3D Multiphysics Sim template. Set the Solver to Simcenter 3D Multiphysics and set the Analysis Type to Structural.	Adding time points to a structural solution to match a reference 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 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)
6.	Enable geometric or material nonlinear effects.	To model geometric nonlinear effects for the thermal-structural solution steps, in the Solution dialog box, on the Solution Control page, select Large Displacements.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
7.	Specify the stress-free reference temperature for the structural solver.	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
8.	Request the types of results to output.	The Structural Output Request modeling object specifies the types of results to recover from the solution (for example, displacements, stresses, and so on).You can specify structural output request both for the solution and for individual solution steps.	Requesting structural output for Simcenter 3D Multiphysics
9.	Create structural solution steps.	Create solution steps as necessary. The end times of your solution steps should correspond to the time steps in the thermal solution results. For the time-assigned temperature data, Simcenter Nastran will interpolate the nodal temperatures when you define times between the time points in the thermal results. However, if a solution step time is outside the thermal time data range, the solver will use the data at the closest time point and will write a warning to the f06 file.	Create or modify a solution step or subcase
10.	Create additional time steps to match thermal solution.	You can add additional time points to the solution automatically by creating an Augmented Time Step List modeling object that references the .bun file that contains the thermal results. You create this modeling object on the Solution dialog box on the Solution Control page.	Adding time points to a structural solution to match a reference solution
11.	Exclude elements from structural analysis.	Use a Deactivation Set to exclude any elements that you don’t want to include in the structural analysis.	Deactivation Set
12.	Create a temperature load in the structural solution.	In the structural solution, create a Temperature Load type of Temperature Set. In the temperature set, create an External Time-Assigned type of Temperature load that references the .bun file that you generated from the thermal solution.	Load setsTemperature
13.	Add constraints, loads, glue, and contact.	Add thermal and structural constraints and loads in the simulation file. Loads can be static or time assigned.	Boundary conditionsUsing fields and expressions to define boundary conditionsSimcenter 3D Multiphysics boundary conditions
14.	Add contact and glue conditions.	Add glue and contact conditions to the model as needed.	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)Contact and glue overview (Simcenter Nastran, Simcenter 3D Multiphysics)
15.	Solve the structural solution.	Solve the structural solution to calculate items such as thermal expansion and temperature-dependent material properties.	Solve the model

Learn more

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

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: structural solution using one-way coupling of temperature loads, 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 } });