Results file and solver files created by a Mapping solution

When you solve an analysis with a Mapping solution type, the mapped results are written to a bun file, [simulation_name]-[solution_name].bun. You can post process this file using this software.

You can also write the following solver specific files in the simulation directory:

• [simulation_name]-[solution_name]_nastran.dat for the Nastran solver

• [simulation_name]-[solution_name]_ansys.inp for the ANSYS solver

• [simulation_name]-[solution_name]_abaqus.inp for the Abaqus solver

• [simulation_name]-[solution_name]_tmg.tempf and [simulation_name]-[solution_name]_tmg.gtempf for the thermal solver in Simcenter 3D Thermal/Flow, Simcenter 3D Electronic Systems Cooling, and Simcenter 3D Space Systems Thermal.

These solver specific files are used as input files by their respective solvers.

Note:

In the Simcenter 3D Multiphysics solver environment, the mapping solver generates only the bun file. Solver specific files are not generated.

The mapping algorithm considers your defined nodes and elements. You can categorize them into target nodes, target elements, transverse gradient target nodes, and transverse gradient target elements. Based on this categorization, the software writes the appropriate cards for the selected solver.

Target nodes

Nodes that you define in the Destination Nodes group in the Mapping Target Set dialog box. When you do not define Mapping Target Set constraints in your target mapping solution, the software recognizes all nodes in the target model as target nodes.

Target elements

Elements that you define in the Destination Elements group in the Mapping Target Set dialog box. When you do not define Mapping Target Set constraints in your target mapping solution, the software recognizes all elements in the target model as target elements.

Transverse gradient target nodes

A subset of target nodes that you define in the Destination Nodes group in the Transverse Gradient Target Zone dialog box.

Transverse gradient target elements

A subset of target elements that you define in the Destination Elements group in the Transverse Gradient Target Zone dialog box.

Results output file

The following mapping results are written to [simulation_name]-[solution_name].bun in base units of the target model, which, for temperature, is either Celsius or Fahrenheit.

Thermal mapping results

• For every target node and every node of a target element, the software writes the nodal temperature, Tnode.

• For every transverse gradient target node, the software writes the nodal temperature, Tnode, and the nodal gradient, ΔTnode

• For every transverse gradient target element: the elemental temperatures, Telement, top and Telement, bottom , and the elemental gradient, ΔTelement.

If the source model does not have transverse gradient results on the multi-layer shells, the values are calculated as follows:

• Tnode = (1 – d/t) ∙ Tnode, bottom + d/t ∙ Tnode, top

• ΔTnode = (Tnode, top –Tnode, bottom)/t

• Telement = (1 – d/t) ∙ Telement, bottom + d/t ∙ Telement, top

• ΔTelement = (Telement, top –Telement, bottom)/twhere t is either:The specified thickness on the transverse gradient pair, and d is t/2. Note: You specify the thickness in the source model in the Transverse Gradient Zone mapping constraint. From the Thickness Option list, select Specify and enter the thickness in the Thickness Value box.The thickness that comes from the source model. In this case, t is the distance between the top and bottom sides of the transverse gradient pair, and d is the distance between the bottom side element of the transverse gradient pair and the transverse gradient target element. Note: You specify the thickness in the source model in the Transverse Gradient Zone mapping constraint. From the Thickness Option list, select From Thermal Model.

If the source model does have transverse gradient results on the multi-layer shells, the elemental and nodal temperature and gradients are directly mapped from the source model to the target model. For Telement, the average of the top and bottom temperatures of the shell layers is used for the mapping. 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 mapping results

• For every target node and every node of a target element, the software writes the nodal contact force and the nodal contact pressure.

Note:

In the Multiphysics solver environment, only temperature results are written in the bun files. Transverse gradient and pressure results are not supported.

Nastran input file

The following cards are written to the [simulation_name]-[solution_name]_nastran.dat Nastran input file.

Thermal mapping results

• For every target node, every node of a target element, and every transverse gradient target node, the TEMP card is written to the Nastran deck.TEMP, , , : the load set identification number: the node number: the nodal temperature

• For every transverse gradient target element, the TEMPP1 card is written to the Nastran deck.TEMPP1, , , , , , : the load set identification number: the element number: the element’s temperature, Telement, which is mapped to the element’s center of gravity: the elemental linear thermal gradient, ΔTelement: the bottom element temperature, Telement, bottom: the top element temperature, Telement, topNote: For transverse gradient target elements associated to multi-layer shells with transverse gradient results in the source model, and are omitted.For transverse gradient target nodes, the TEMPP1 card is not written to the Nastran deck.

Flow mapping results

• For every target node and every node of a target element, the FORCE card is written to the Nastran deck.FORCE, , , , , , : the load set identification number: the node number: the magnitude of the force vector, , : the normalized components of the force vector

ANSYS input file

The following cards are written to the [simulation_name]-[solution_name]_ansys.inp ANSYS input file.

Thermal mapping results

• For every target node, every node of a target element, and every transverse gradient target node, the BF card is written.BF,  , TEMP, : the node number: the nodal temperature

• For every transverse gradient target element, the BFE card is written.BFE,  , TEMP, 1, , , ...,  BFE,  , TEMP, M+1, , , ..., : the element numberM+1: M is the number of nodes in the element.: the bottom elemental temperature for the Nth node, TN, bottom: the top elemental temperature for the Nth node,TN, topNote: For transverse gradient target elements that are associated to multi-layer shells with transverse gradient results in the source model, the BFE card is not written.For transverse gradient target nodes, the BFE card is not written to the ANSYS input file.Transverse gradient results are supported only on SHELL181 elements.

Flow mapping results

• For every target node and every node of a target element, the F card is written:F, , FX,  F, , FY,  F, , FZ, : the node number, , : the components of the force vector

Abaqus input file

The following cards are written to the [simulation_name]-[solution_name]_abaqus.inp Abaqus input file.

Thermal mapping results

• For every target node and every node of a target element:*TEMPERATURE , Temperature: the nodal temperature

• For every transverse gradient target node:Temperature , , : the node number: the nodal temperature, Tnode: the nodal linear thermal gradient, ΔTnode*Note: For transverse gradient target elements, nothing is written to the Abaqus input file.

Flow mapping results

• For every target node and every node of a target element:*CLOAD , 1, <Load 1> , 2, <Load 2> , 3, <Load 3>: the node numberLoad 1, Load 2, Load 3: the components of the force vector

Thermal input file

When you perform thermal mapping, the following data is written to the [simulation_name]-[solution_name]_tmg.tempf and [simulation_name]-[solution_name]_tmg.gtempf files for the thermal solver.

• For every target node and every node of a target element, the [simulation_name]-[solution_name]_tmg.gtempf file contains:, : the element number: the nodal temperature

• For every target element and every element that has all its nodes belonging to the target node list, the [simulation_name]-[solution_name]_tmg.tempf file contains:, : the element number: the elemental temperature

How do I

Map thermal or flow results to another model

Update mapping constraints in the source model

Define mapping options

Learn more

Mapping results data to another model

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

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

Related Topics

Mapping constraints

Results file and solver files created by a Mapping solution, 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 } });