Aeroelastic divergence analysis workflow (SOL 144)

Step	Summary	Detailed help topic
1.	Create the FEM and Simulation	In the New FEM and Simulation dialog box, set the solver to Simcenter Nastran and the analysis type to Aeroelastic.
2.	Specify the Simcenter Nastran solution	In the Solution dialog box, set the solution type to SOL 144 Static Aeroelastic Response and clear the Automatically Create Step or Subcase check box.Note: You create a divergence subcase later in the workflow.
3.	Idealize the part geometry	In the idealized part file, perform any necessary part idealizations.
4.	Construct the FE structural model	In the FEM file, create the FE representation of the structure. Define the structural mesh, material properties, and so on as you would for any other structural solution type.
5.	Mesh the aerodynamic surfaces	In the FEM file, use the Aero Panel command to mesh the aerodynamic surfaces with aero panels.Create an aero panel mesh for each aerodynamic surface. That is, create a distinct aero panel mesh for each wing, aileron, horizontal stabilizer, elevator, and so on.Note: You can also use the Aero Body command to mesh aerodynamic bodies such as fuselages, external tanks, and so on.	Create a mesh of aero panelsCreating aerodynamic panel meshesCreating aerodynamic body meshes
6.	(Optional) Create sets of structural nodes	In the FEM file, in preparation for interfacing the structural model with the aerodynamic surfaces, use the New Group command to create structural node sets. Create a set of structural nodes for each aerodynamic surface.Note: Although this step is optional, it allows you to avoid having to select the structural nodes individually when you create the splines.
7.	Interface the structural model with the aerodynamic surfaces	In the Simulation file, use the Aero Spline command to create splines that relate the motion of the structural model to the motion of the aero model.Create one or more aero splines for each aero panel and aero body mesh.	Create an aero splineSpline options
8.	Define the static aerodynamic parameters	In the Simulation file, create an aerodynamic static parameters modeling object that defines the rigid body coordinate system, reference chord length, reference span, reference wing area, and, if applicable, symmetry plane.
9.	Assign modeling object to the solution	In the Simulation file, assign the static aeroelastic parameters modeling object to the solution.	Assign a modeling object to a solution or solution subcase
10.	Create a divergence subcase	In the Simulation file, create an aeroelastic divergence subcase.	Create an aerodynamic divergence subcase
11.	Define divergence data	In the Simulation file, create an aerodynamic divergence data modeling object to specify the number of roots desired and the Mach numbers at which to perform the divergence analysis.	Define aerodynamic divergence data
12.	Define complex eigenvalue extraction parameters	In the Simulation file, create a complex eigenvalue modeling object to specify the extraction method, number of roots desired, and so on.
13.	Assign modeling objects to the subcase	In the Simulation file, assign the aerodynamic divergence data and complex eigenvalue modeling objects to the divergence subcase.	Assign a modeling object to a solution or solution subcase
14.	Constrain the model	In the Simulation file, create constraints for the model and add them to the constraint containers in the divergence subcase.
15.	Specify miscellaneous parameters	In the Simulation file, edit the static aeroelastic response solution to turn on the AUTOSPC parameter and set the OPPHIPA parameter to 1.
16.	Solve the model	The Solution Monitor contains information about the status of your solution, and the Simcenter Nastran .f06 output file contains the requested results from your analysis.To locate the Simcenter Nastran .f06 file, right-click the solution and select Browse.
17.	Review the results	Open the .f06 file to view the divergence analysis results.

How do I

Assign a modeling object to a solution or solution subcase

Define an aerodynamic control surface

Create a static aeroelastic subcase

Define aerodynamic divergence data

Create an aerodynamic divergence subcase

Create a fictitious support

Plot trim conditions

Learn more

Static aeroelastic response analysis (SOL 144)

Aeroelastic trim analysis workflow (SOL 144)

Defining trim variables

Constraints in trim analysis

Post-processing aeroelastic trim analysis results

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Aeroelastic divergence analysis workflow (SOL 144), 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 } });