Aeroelastic trim 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 aeroelastic trim subcases 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.	(Optional) Create coordinate systems to define hinge lines of control surfaces	In the FEM file, in preparation for defining control surfaces, for each control surface, create a coordinate system whose Y-axis is the hinge line for the control surface.Note: Although this step is optional, it allows you to avoid having to create the coordinate systems when you define the hinge lines of the aerodynamic control surfaces.
8.	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
9.	Define the aerodynamic control surfaces	In the Simulation file, use the Aerodynamic Control Surface command to define the aerodynamic control surfaces.	Define an aerodynamic control surface
10.	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.
11.	Assign the modeling object to the solution	In the Simulation file, edit the static aeroelastic response solution to assign the aerodynamic static parameters modeling object to the solution.	Assign a modeling object to a solution or solution subcase
12.	Create trim subcases	In the Simulation file, create a static aeroelastic subcase for each trim condition that you want to simulate.	Create a static aeroelastic subcase
13.	Define the trim conditions	In the Simulation file, use the Trim Variables Manager command to:Define the Mach number and dynamic pressure at which to perform the analysis.Specify the trim analysis type.Define the trim variables to include in the analysis.Assign values to trim variables.Link trim variables.	Defining trim variables
14.	Create a fictitious support	In the Simulation file, edit the static aeroelastic response solution to define a fictitious support.	Constraints in trim analysisCreate a fictitious support
15.	Constrain the model	In the Simulation file, if applicable, create constraints for the model and add them to the constraint containers for each subcase.	Constraints in trim analysis
16.	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.
17.	Create output requests	In the Simulation file, edit the static aeroelastic response solution to request output such as aerodynamic pressures, displacements, grid point forces, and so on.
18.	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.
19.	Post-process the results	Use the post-processing commands to create contour plots of structural and aerodynamic results such as displacement, stress, strain, aerodynamic pressure, and so on.Use the Trim Analysis Results post-processing scenario to plot trim analysis results such as trim variable values, stability and control derivative coefficients, and so on.	Post-processing aeroelastic trim 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 divergence 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 trim 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 } });