Deterministic workflow for external enforced motion loading

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

Step	Summary
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, and typing a name for the solution process.A node with this name appears in the Simulation Navigator.
2.	Import a result file.	Use the Input File dialog box to import an external result file that contains an associated mesh and the following time or frequency-dependent loads:Stationary vibration loads (displacements, velocities, or accelerations) at the fluid-structure interface.Vibration loads (displacements, velocities, accelerations, or forces) at the fluid-structure interface from a rotating mesh.Note: The vibration loads can have translational or rotational degrees of freedom.The input file must be in a supported format, such as ANSYS RST, Abaqus ODB, and Simcenter Samcef DES.Note: You must upgrade Abaqus files saved with a previous version of Abaqus to a new version of Abaqus with the upgrade options in the Options group.For information on the available upgrade options, see Define Data Source dialog box (external 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 Enforced Motion 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 the import of the result file, you can:Visualize the associated mesh, also known as intermediary mesh, with the right-click command Load Intermediary Mesh on the Input File node in the Simulation Navigator.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 the units in the Unit System 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 and navigate through different frequencies or time steps.
5.	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 other software for further processing.
6.	Map the result data from a source to a target mesh	Edit the Mesh Mapping Data node to map regions between meshes.For more information, see Mapping of result data between meshes.
7.	Transform time dependent loads into the frequency domain.	Use the Time Signal Processing command to convert input loading from time to frequency domain and limit the number of results files when you specify lower and upper samples. When the input loading is already in frequency domain, you can proceed to step 9.For more information on time to frequency domain conversion, see Transforming time-domain to frequency.
8.	Convert imported data to binary format	Use the Export to Binary File command when it is available to convert the imported data to a Simcenter HDF5 Data File (*.sc_h5) in binary format.Note: This command appears when no other Add Operation commands, such as Mesh Mapping, Time Signal Processing, and so on, were previously executed.Other Add Operation commands already include the instruction to write an HDF5 file in binary format.
9.	(Optional) Validate the setup.	Use the Validate command to validate the setup of the solution process. Validation results are displayed in the Information window.
10.	Solve the solution process.	Process the solution process with the Solve command.For more information on the solving process, see Solving the solution process.
11.	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 displacement, velocity, and acceleration 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.For information on creating a post-processing view, see Create and edit post-processing scenarios.
12.	Extract vibrations and apply to nodes.	For the Simcenter Nastran solver, extract the vibrations stored in the HDF5 result file and apply them to target nodes by using:The Create Load Recipe from Results command.You use this command instead of, for example, the Enforced Motion 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 such load recipe.Note: When you attach the load recipe to an active solution or update a solution from the load recipe, make sure to choose the load condition type File Reference.For information on creating a load recipe from results, see Create a load recipe from solution process results.The Enforced Motion from External File command. You enter the path to the HDF5 result file, choose the Subcase, and infer the Data Set with the Infer Data Set button.For more information, see Enforced motion loads from external files.

Learn more

External enforced motion loading

Mapping of result data between meshes

Load recipes

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 enforced motion 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 } });