Thermal/Flow, Electronic Systems Cooling, and Space Systems Thermal > Mapping

Mapping results data to another model

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

You map thermal or flow analysis results to the target model working in the target model Simulation file, where you create Simcenter 3D Thermal/Flow, Simcenter 3D Electronic Systems Cooling, or Simcenter 3D Space Systems Thermal solutions with the Mapping analysis type, called the mapping solution.

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, flow, or coupled thermal-flow solution with results	FEMSimulation fileMapping solutionStructural, thermal, flow, or coupled thermal-flow solution

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 Temperature 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.

Transverse temperature gradients

You can also map transverse temperature gradients between two sets of elements in two closely spaced parallel regions or through multi-layer shell elements of the source model to a shell region of the target model. To map transverse temperature gradients, you must create:

A Transverse Gradient Zone type of Mapping constraint in your source solution.
A corresponding Transverse Gradient Target Zone constraint in your target mapping solution.

When you map results from two-parallel 2D meshes to one 2D target mesh, the source temperature gradient is defined by the difference between the top layer temperature and the bottom layer temperature, divided by the thickness. The gradient is mapped to the corresponding nodes and elements of the target model.

When multi-layer shells in the source model have transverse gradient results, the results are mapped directly from the source model to the target model. You must select the Transverse Temperature Gradients results set in the source model to get the Transverse Temperature Gradients – Elemental and Transverse Temperature Gradients – Nodal results after the analysis is complete.

Flow forces

The flow mapping solution creates an association between each node or element centroid of the target model and its closest element in the source model.

If the target node is located inside the associated element, its pressure and shear stress is interpolated using the nodal pressures and shear stress of all nodes of the associated element, including mid-side nodes for parabolic elements.
If the target node is located outside the associated element, its pressure and shear stress is extrapolated using the nodal pressures and shear stresses of all nodes of the associated element, including mid-side nodes for parabolic elements.You can define pressure extrapolation options while you map flow results to the target model. You can:Limit the extrapolation to the pressure range of the source model or to the pressure range of each element of the source model.Set no limit to the pressure extrapolation.You can also specify a pressure offset to be applied to the mapped pressures.

To get the nodal fluid dynamic force, the flow mapping solution multiplies the mapped pressure and shear stress by a bounding area around each node in the target model. The bounding area around each node is determined by connecting the midside points of the surrounding element edges and the centroids of the surrounding elements.

The nodal fluid dynamic forces represent force vectors that the flow exerts on its boundary surfaces in the target model.

Mapping output

The software writes mapped temperatures, mapped transverse temperature gradients, or mapped forces to a results file ([simulation_name]-[solution_name].bun) which can be used to view the mapping result in post processing, or included in a Simcenter Nastran simulation as a preload.

The software can output the results of the mapping as a solver input file in Nastran, ANSYS, Abaqus, Thermal/Flow, Electronic Systems Cooling, or Space Systems Thermal.

The software can also automatically create a complete solution with all the appropriate steps, subcases, and loads defined for Nastran, ANSYS, and Abaqus solvers. The mapping solver creates the following solutions:

SOL 101 Linear Statics—Global Constraints for Simcenter Nastran only
Linear Statics for ANSYS
General Analysis for Abaqus

You can create more than one solution at the same time, such as one for both Simcenter Nastran and ANSYS. In that case, the mapping solver creates one set of loads that is shared between the solutions.

When you automatically create a structural solution, mapped transverse temperature gradient results are not included in the loads. Instead, you must use user defined text that points to the appropriate solver input file. In Simcenter Nastran, you can also append the transverse temperature gradient data from the Nastran solver input file to your Simulation file using the File→Append and Merge Entities commands.

Axisymmetric thermal mapping

When your source model contains mixed axisymmetric and non-axisymmetric elements, to ensure that the 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.

The following table shows the type of mapping solution that you must select from the Analysis Type list in the Solution dialog box. The analysis type depends on the type of source and target models that you have.

Type of source model	Type of target model	Mapping solution type
Full 3D	Full 3D	Mapping
Full 3D	Axisymmetric	Axisymmetric Mapping
Axisymmetric	Full 3D	Mapping
Axisymmetric	Axisymmetric	Axisymmetric Mapping

Example:

The following graphic shows temperature mapping from an axisymmetric source model to a 3D target model using the Mapping solution type.

The image on the left shows the temperature on 2D elements that model the thermal analysis on an axisymmetric light bulb.
The image on the right shows the same temperatures mapped on the tetrahedral elements of a full light bulb.

How do I

Map thermal or flow results to another model

Update mapping constraints in the source model

Define mapping options

Learn more

Customizing a Nastran input file with user defined text

Customizing Abaqus input files with user-defined text

Customizing ANSYS input files with user defined text

Look up more details

Results file and solver files created by a Mapping solution

Transverse gradient mapping

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Simcenter 3D Thermal/Flow, Electronic Systems Cooling, and Space Systems Thermal boundary conditions