Deterministic workflow for external 2D electromagnetic force loading

Before you perform the Model and Load Pre-processing task, a Simulation file must be the work and displayed part.

Step	Summary	Detailed steps
1.	Create the solution process.	In the Simulation Navigator, create a new Model and Load Pre-processing solution process by right-clicking a simulation node→New Solution Process→Model and Load Pre-processing→type a name for the solution process. A node with this name appears in the Simulation Navigator.	Create solution process
2.	Import a result file.	Use the Input File dialog box to import an external result file that contains a 2D mesh and associated forces from an electromagnetic simulation. For example, the associated mesh represents the part of the mesh boundaries where the electromagnetic software exported the data. The input file must be an ASCII universal file (.unv) or other supported file.
3.	Select the data types to be processed.	Click the Refresh icon to populate the data from the imported files to the fields in the data table. After the software populates the data, you can access and change the Target Storage Name. Unique target storage names let you track different loads, for example, in the HDF5-specific Data Set field of the Force from External File dialog box and Data definition in the Scenario Based Data-Visualization Navigator or Editor subpanel.
4.	Visualize imported results and an associated mesh.	After you import the result file, you can:Visualize the associated mesh, also known as intermediary mesh, by right-clicking the Input File node in the Simulation Navigator and choosing Load Intermediary Mesh.Note: If necessary, use the Fit command to see the entire intermediary mesh in the work view.If you go back to step 2, load a different result file, or change any values in the Options group of the Input File dialog box, the software unloads the intermediary mesh.Generate a contour plot of the results with a preconfigured post-processing view in the Scenario Based Data-Visualization navigator.	Visualize the input files
5.	Extrude the forces and free element edges.	Use the Load Extrusion command to extrude the free element edges of the 2D mesh and its applied loads.	Load Extrusion dialog box
6.	(Optional) Validate the setup.	Use the Validate command to validate the setup of the solution process. Validation results are displayed in the Information window.
7.	Solve the solution process.	Process the solution process with the Solve command.	Solving the solution process
8.	Visualize the preprocessed results.	Use a preconfigured post-processing view to generate a contour plot of the pre-solver results and navigate through different time steps.You can display nodal force results and the extruded mesh.	Create and edit post-processing scenarios
9.	Transfer mesh and load information.	You must use the Mesh Mapping command when you want to further process the mesh and load information of the result file in Pre/Post.Optionally, you can instruct the software to write the mesh mapping matrix to use it in another software for further processing by using the Export Mesh Mapping Matrix check box and selecting a file for export.
10.	Map the result data from a source to a target mesh	Edit the Mesh Mapping Data node to map regions between the 2D extruded mesh and, for example, a 3D structural mesh. You typically use the Conservative Maximum Distance method when you map 2D electromagnetic analysis result data between meshes.	Mapping of result data between meshes
11.	Transform time-dependent loads into the frequency domain.	Use the Time Signal Processing command to convert input loading from time to frequency domain. When the input loading is already in frequency domain, you can proceed to the next step.Note: If you used the File Loading option in the Input File dialog box to limit the number of results files to import, you can further limit the results files when you specify lower and upper samples with the Time Signal Processing command.	Transforming time-domain to frequency
12.	(Optional) Validate the setup.	Use the Validate command to validate the setup of the solution process. Validation results are displayed in the Information window.
13.	Solve the solution process.	Process the solution process with the Solve command.	Solving the solution process
14.	Visualize the preprocessed results.	Use a preconfigured post-processing view to generate a contour plot or XY plot of the pre-solver results and navigate through different time steps.You can display nodal force results.If you specified influencing nodes (number of nodes to be considered within the maximum search distance) during the mesh mapping step, you can verify the quality of the mesh mapping by inspecting the vectors of NumInfluencingNodes on Nodes data set in a contour plot.	Create and edit post-processing scenarios
15.	Extract nodal forces and apply to nodes.	For the Simcenter Nastran solver, extract the forces stored in the HDF5 result file and apply them to target nodes by using one of the following commands:Create Load Recipe from Results.You use this command instead of the Force from External File command, when the HDF5 file contains multiple load cases, because in a solution the software can easily create subcases for these load cases from this type of load recipe.Note: When you attach the load recipe to an active solution or update a solution from the load recipe, be sure to choose the load condition type File Reference.Force from External File. You enter the path to the HDF5 result file, choose the Subcase, and infer the Data Set by clicking Infer Data Set.	Create a load recipe from solution process resultsForce or moment loads from an external file

Learn more

Transform pre-computed 2D electromagnetic forces into loads

Mapping of result data between meshes

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Deterministic workflow for external 2D electromagnetic force loading, 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 } });