Rotor dynamic superelement analysis workflow (SOL 414,103)

The workflow for a rotor dynamic superelement analysis involves the following:

• Generating the superelement for the rotor.

• Using the generated rotor superelement in a rotor dynamic analysis.

• Validating the superelement.

The workflows for generating and using the rotor superelement are outlined below.

Generate the rotor superelement

In this workflow, you prepare your 1D, 2D axisymmetric, or 3D model of the rotor by defining the rotor, identifying the nodes to retain in the generated superelement, and optionally adding damping and boundary conditions.

Note:

If the model of the rotor is already created, save it as a standalone component (that is, remove it from the assembly FEM file), and remove boundary conditions, bearings, stators, and other rotors. Only the rotor objects of the rotor region should be defined.

If the model has multiple rotors, you must create a superelement for each rotor separately.

Step	Summary	Detailed help topic
1.	For the rotor part, create the FEM and Simulation files.	In the New FEM and Simulation dialog box, set the following:Solver to Simcenter Nastran****Analysis Type to Rotor Dynamics.For a 2D axisymmetric model, 2D Solid Option to the plane and axis of revolution for the model.	Create new FEM and Simulation files
2.	Specify the Simcenter Nastran solution.	In the Solution dialog box, set Solution Type to SOL 414,103 Eigenvalues and Superelement Reduction. After you click Create Solution, from the Computation Options list, select Superelement Reduction.Note: Do not use a comma (,) or special characters such as @ and & in the solution name. Underscores (_) are acceptable.	Create or modify a solution
3.	If your rotor model is not already created, idealize the part geometry.	In the idealized part file, perform any necessary part idealizations.For example, to create a 2D axisymmetric model of the rotor, you may need to do the following:Align the center of rotation and the radial axis of the axisymmetric portion of the part to the absolute coordinate system.Split or stitch the rotor part.	Idealize geometryPositioning the model in an axisymmetric environment in Axisymmetric analysisModeling symmetry using coupled degrees of freedom
4.	If your rotor model is not already created, construct the FE model.	In the FEM file, create the FE representation of the model.Create a mesh for the rotor. In this mesh, make sure that nodes are located on the axis of rotation of the rotor where bearings are located.For a 2D axisymmetric model of the rotor, use axisymmetric elements. To link the 2D nodes to nodes on the rotor axis where lumped pass, forces, boundary conditions, and bearings are to be defined, use the FOU3 coupling element.For a 3D model of the rotor, you can use any elements except axisymmetric elements.	MeshingModeling axisymmetry (SOL 414)
5.	Create rotor regions.	Use the Define Rotor Region command to select the FE entities that comprise the rotor model. You can do this by selecting elements or meshes directly, or indirectly by selecting parent geometric entities.Note: You must define the rotor axis along the Z-axis. If you are not using the absolute coordinate system, use the local coordinate system that you defined.	Create a rotor region
6.	Define the rotors.	Use the Rotor Modeling Assembly command to select the rotors to use in the solution.	Define a rotor
7.	Create the retained nodes.	To create a retained node, select a node on the rotor and apply the Fixed Boundary Degrees of Freedom or Free Boundary Degrees of Freedom constraint.	Defining the nodes to retain in Rotor dynamic analysis with superelements (SOL 414,103)
8.	Set the reference frame.	Set the reference frame in the Solution dialog box on the Bulk Data page. How you set the reference frame depends on the symmetry of your rotor and how you want to apply damping. If the rotor is unsymmetric, you must use the rotating frame .If the rotor is symmetric, you generally use a fixed reference frame, but you can also use a rotating frame.The reference frame also determines where you can take damping into account.If you use a fixed frame, you can take damping into account during the creation of the superelement.If you use a rotating frame, you can take damping into account during the use of the superelement.	Setting the reference frame and applying damping in Rotor dynamic analysis with superelements (SOL 414,103)
9.	(Optional) Define the damping.	If the reference frame is fixed, define the damping in the Solution dialog box, on the Parameters page.	Setting the reference frame and applying damping in Rotor dynamic analysis with superelements (SOL 414,103)
10.	Set the eigenvalues to compute for Subcase - Eigenvalues and Superelement.	For a 2D axisymmetric or 3D model of the rotor, set the following for the Real Eigenvalue - Lanczos modeling object.Frequency rangeEnsure that the upper limit of the frequency range is two times the highest frequency of the rotor rotation.Number of modes to computeNote: Requesting too many modes relative to the number of retained nodes can yield redundant static and normal modes with singular stiffness matrices, which can cause the size of the rotor superelement to be larger than the rotor model.	Specifying eigenvalues in Rotor dynamic analysis with superelements (SOL 414,103)
11.	(Optional) Create and configure additional subcases.	In addition to Subcase - Eigenvalues and Superelement, you can create the following subcases:Subcase - Static Loads****Subcase - Transient Preload	SOL 414,103 superelement analysis in Rotor dynamic analysis with superelements (SOL 414,103)
12.	(Optional) Define the loads for the preload subcase.	If you added a preload subcase, choose from the loads in the Rotor Dynamics tab, Loads and Conditions group, Load Type list.
13.	Assign the modeling objects to the solution.	If you created the modeling objects independent of the solution, assign them to the solution. For example, your model might use the following modeling objects: Real Eigenvalue - LanczosFourier HarmonicsGlobal Nonlinear Control ParametersOutput requests	Create a modeling objectAssign a modeling object to a solution or solution subcase
14.	Post-process the results.	Use the post-processing commands to view the rotor dynamics analysis results. Note: To validate your model, define the same boundary conditions, bearings, and forces as in the original model and compare the results. The results should be the same.	Post-processing
15.	Validate the rotor superelement.	Create and solve SOL 414,103 eigenvalue analysis, and compare the results with the results from the generated superelement in step 14.The results of both solutions should provide the same modes. When the results match, the rotor superelement is ready to be added to an assembly FEM file for the full model, as outlined in the next workflow.	Validating the generated superelement in Rotor dynamic analysis with superelements (SOL 414,103)

Use the rotor superelement in a rotor dynamic analysis

In this workflow, you add the superelement to an assembly FEM, define the rotor, and add the bearing connections and boundary conditions to the retained nodes before solving the full model. You can start with:

• An existing assembly FEM file in which you will replace a component FEM with its superelement representation.

• A new assembly FEM file in which you will add a new component FEM that you replace with its superelement representation.

Step	Summary	Detailed help topic
1.	If necessary, create an assembly FEM (.afm) file.	In the New FEM and Simulation dialog box, set the solver to Simcenter Nastran and the analysis type to Rotor Dynamics.	Create an assembly FEM file
2.	If necessary, add a new component FEM (.fem) file.	Right-click the .afm file and choose Add New Component.In the New Part File dialog box, select Simcenter 3D Rotor Dynamics.	Add a new FEM to an assembly FEM
3.	Replace the component FEM file with the superelement.	When you add the rotor superelement to the model, you can convert the units to match those used in the assembly FEM file, set damping, and set scaling factors for the matrices.You can replace as many component FEM files with the rotor superelement as necessary.	Replace a component FEM with superelements (SOL 414)
4.	If necessary, create the Simulation file and specify the Simcenter Nastran solution.	Right-click the .afm file and choose New Simulation.In the New Part File dialog box, select Simcenter 3D Rotor Dynamics.In the Solution dialog box, set the solution type to any of the SOL 414 solutions except for SOL 414,101 Maneuvers, depending on what you want to accomplish in the analysis.Note: To be able to recover superelements, set Generate Restart Point (RSTGEN) to Yes in the Global Nonlinear Control Parameters modeling object.
5.	Create the rotor region.	For the rotor superelement, use the Define Rotor Region command by selecting all of the retained nodes.	Create a rotor region
6.	Create a new coordinate system with its Z-axis pointing in the direction of the rotation axis of the rotor superelement.	The Z-axis of a rotor always defines the direction of rotation of the rotor, so the coordinate system of the original rotor and the superelement rotor must be consistent. If the rotor rotation axis of the superelement is not oriented in the Z direction, create a local coordinate system that is consistent with the original rotor.	Create coordinate systems
7.	Define the rotor.	Use the Rotor Modeling Assembly command to select the rotors to use in the solution.You can solve models with up to 10 superelement rotors.	Define a rotor
8.	With the assembly FEM file as the work and displayed part, create coincident nodes.	In preparation for creating bearing connections, create coincident nodes on the retained nodes on the rotor axis where bearings are located.	Create nodes
9.	Create the CBEAR2 or bearing connections and CBUSH2 bearing supports.	You can create the bearing and bushing connections using 1D connections or bearing universal connections.Define the bearing elements between each set of coincident nodes.	Create connection elements between coincident nodes with CBEAR2 elementsBearing universal connection for rotor dynamics (SOL 414)Using bushing universal connections in rotor dynamics (SOL 414)Create and edit universal connectionsRealize (mesh) universal connections
10.	Assign properties to the bearing elements.	Assign mechanical and physical properties to the bearing elements.	Define rotor bearing or bushing properties
11.	Define the rotational speed for bearing elements.	Note: This step applies to CBEAR2 and CBUSH2 elements. It is only required when the stiffness, damping, or mass matrices for a CBEAR2 or CBUSH2 element are speed-dependent.When required, use the Define Rotor Connections Assembly command to specify the rotational speed for CBEAR2 or CBUSH2 elements.
12.	Create RBE2 spider elements.	To connect a bearing element to the mesh of the stationary portion of the model, use an RBE2 spider element. For the independent node of the RBE2 element, select a node in the connectivity of the bearing element that is not in the mesh of the rotor.To connect a bearing element to ground, constrain the displacements in the plane normal to the axis of rotation of the node in the connectivity of the bearing element, but not in the mesh of the rotor.	Working with RBE2 and RBE3 spider elements
13.	Define rotor dynamic solution parameters.	Create a Rotor Dynamics Solution Parameters modeling object to specify parameters for the rotor solution. Reference System (REFSYS) must be set the same as in the original rotor superelement.For example, if the rotor superelement is created with a fixed reference frame, the analysis in which the superelement is used must also use a fixed reference frame.Rotor speed settings depend on the solution type.	Define the rotor dynamics solution parametersSpecifying rotor speeds in Rotor dynamic analysis (SOL 414)
14.	Assign the modeling objects to the solution.	Edit the solution to assign the rotor dynamics solution parameters modeling object to the solution.	Assign a modeling object to a solution or solution subcase
15.	If you are using the superelement in a static preload subcase, define the angular motion in the rotating reference frame.	Use the Rotation command to specify the angular velocity and angular acceleration that the model is undergoing.	RotationDefine a rotation load
16.	Solve the rotor dynamics model.	The Solution Monitor contains information about the status of your solution.	Solve the modelSolution Monitor
17.	Post-process the results.	Use the post-processing commands to view the rotor dynamics analysis results. Save the results so that you can validate them with the original model.	Post-processingRecover superelements (SOL 414)
18.	Validate the results of the analysis.	Ensure that the rotor superelement is in the same configuration as the original model (for example, use the same forces, same connection elements, and so on). Solve the original model, and compare the results that you saved in step 17. The results of the solutions for both models should be very similar.

Rotor dynamic superelement analysis workflow (SOL 414,103), 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 } });