Deterministic workflow for external pressure loading

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

Note:

For a workflow that supports turbulent boundary layer creation see Stochastic workflow for turbulent boundary layer loading.

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→type 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 pressure loads and an associated mesh. For example, the associated mesh represents the part of the CFD mesh boundaries, where the CFD software has exported the data. The input file must be in the CFD General Notation System (CGNS) or Simcenter Nastran OP2 format.When you choose a CGNS file, you can choose to import:Only the selected file if this is the only file you need for your analysis. For example, for temperature mapping one CGNS file contains all the steady state data.All files associated with the first selected result file if each file represents a time step.Note: The software searches the directory of the previously selected result file and imports all result files that file names match a specific File Name Separator.Subsequent files associated with the first selected result file if each file represents a time step.Note: The software searches the folder of the previously selected result file and imports all subsequent result files that file names match a specific File Name Separator.
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 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 dialog box and navigate through different 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. 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.For more information on time to frequency domain conversion, see Transforming time-domain to frequency.
8.	Convert pressure to force.	Use the Pressure to Force command to convert pressure to nodal forces for later processing by a solver, such as Simcenter Nastran.
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 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.For information on creating a post-processing view, see Create and edit post-processing scenarios.
12.	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:The Create Load Recipe from Results command.You use this command instead of, for example, 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 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 Force 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 Force or moment loads from an external file.

Learn more

External pressure 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 pressure 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 } });