Multiphysics

Mapping results data to another model in Simcenter 3D Multiphysics

Mapping analysis allows mapping of steady state or transient temperatures onto another model with potentially a different mesh. This allows you to transfer temperatures onto a target model, typically an independent structural model of the same geometry. For example, you can include these temperatures in a stress and distortion analysis.

The target FEM must use the same global coordinate system as the source FEM, and both models should be geometrically congruent. However, they need not have the same mesh.

Source model	Target model
FEMSimulation fileThermal solution with results	FEMSimulation fileMapping solutionStructural, thermal, or coupled thermal-structural solution

Note:

If the source thermal model was created in the Simcenter 3D Multiphysics environment, you must use the Mapping solution in the Multiphysics environment. If the source thermal model was created in the Simcenter 3D Thermal environment, you must use the Mapping solution in the Thermal environment.

The mapping process associates a specific element in the source model to each target node or element. This association is based on the closest distance criteria and controlled by the zone associations. The mapping process maps results from the selected solution in the source model to the mapping solution in the target model. The results from the mapping solution can then be used by the target solution as pre-loads or initial conditions.

Aligning source and target models

The mapping solver can automatically align source and target models if you define the following three named points in both models: MAP1, MAP2, and MAP3. The three points in each model must correspond to each other.

Temperatures

Temperature mapping creates an association between each node or element centroid of the target model and its closest element in the thermal model.

If the target node is located inside the associated thermal element, its temperature is interpolated using the nodal temperatures of all nodes of the associated thermal element, including mid-side nodes for parabolic elements.
If the target node is located outside the associated thermal element, its temperature is extrapolated using the nodal temperatures of all nodes of the associated thermal element, including mid-side nodes for parabolic elements. Select a method from the Extrapolation Type list in the Solution dialog box, to specify how you want to restrict the extrapolated temperature.To restrict the extrapolated temperature to the interval between the lowest and highest nodal temperature of the associated thermal element, select Limit to Element Range.To restrict the extrapolated temperature to the interval between the lowest and highest temperature throughout the thermal model, select Limit to Model Range.To leave the extrapolated temperature unrestricted, select Unlimited.

Both the interpolation and the extrapolation algorithms rely on finite elements shape functions.

Mapping output

The software writes mapped temperatures to a results file ([simulation_name]-[solution_name].bun) that can be used to view the mapping result in post processing, or included in a structural solution as a preload.

Axisymmetric thermal mapping

When your source model contains mixed axisymmetric and non-axisymmetric elements, to ensure that this software associates the axisymmetric elements to the desired elements in the target model, you can define one or more Axisymmetry Association Zones in the source model and, for each Axisymmetry Association Zone, a Axisymmetry Target Zone constraint in the target model. Temperatures of axisymmetric elements in the source model are mapped symmetrically around the appropriate axis on the target elements that are not in the axisymmetric plane in the source model.

How do I

Define coupled solution parameters

Learn more

Simcenter 3D Multiphysics overview

Two-way fluid-structure interaction

Defining multiphysics solution steps

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