Rotor dynamic synchronous harmonic response analysis workflow (SOL 414,111)

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 Rotor Dynamics.	Create new FEM and Simulation files
2.	Specify the Simcenter Nastran solution.	In the Solution dialog box, set the solution type to SOL 414,111 Harmonic Response.	Create or modify a solution
3.	Idealize the part geometry.	In the idealized part file, perform any necessary part idealizations.	Idealize geometry
4.	Construct the FE model.	In the FEM file, create the FE representation of the model.As a best practice, create a distinct mesh for each rotor. In this mesh, make sure that nodes are located on the axis of rotation of the rotor where you want to define:BearingsMass imbalance	Meshing
5.	Create coincident nodes.	In preparation for creating bearing connections, create coincident nodes at the nodes in the rotor mesh that are located on the axis of rotation of the rotor where bearings are located.You can create the bearing connections using 1D connections or bearing universal connections.	Create nodes
6.	Create the bearing connections using 1D connections. (Option 1)	Define the bearing elements between each set of coincident nodes.Assign mechanical and physical properties to the bearing elements.Create RBE2 spider elements.To connect a bearing element to the mesh of the stationary portion of the model, use an RBE2 spider element. Use the node in the connectivity of the bearing element that is not in the mesh of the rotor as the independent node for the RBE2 spider element.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.	Create connection elements between coincident nodes with CBEAR2 elementsDefine rotor bearing or bushing propertiesWorking with RBE2 and RBE3 spider elements
Create the bearing connections using universal connections. (Option 2)	Create the bearing universal connections between each set of coincident nodes.Realize (mesh) the universal connections to generate the appropriate CBEAR2 and RBE2 elements.Assign mechanical and physical properties to the bearing elements.	Bearing universal connection for rotor dynamics (SOL 414)Using bushing universal connections in rotor dynamics (SOL 414)Create and edit universal connectionsRealize (mesh) universal connectionsDefine rotor bearing or bushing properties
7.	Constrain the model.	In the Simulation file, define any constraints.If you do not specify an axial stiffness for the bearings, make sure that you constrain the rotor against axial displacement.
8.	Create rotor regions.	For each rotor, 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.	Create a rotor region
9.	Define the rotors.	Use the Rotor Modeling Assembly command to select the rotors to use in the solution.You can solve models with up to 10 rotors.	Define a rotor
10.	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.
11.	Define rotor dynamic solution parameters.	Create a Rotor Dynamics Solution Parameters modeling object to specify parameters for the rotor dynamics solution such as starting speed, step size, number of steps, fixed or rotating reference frame, synchronous analysis, and so on.Note: For detailed information on how to specify starting speed, step size, and number of steps, see Specifying rotor speeds for synchronous SOL 414,111 harmonic response analysis.	Define the rotor dynamics solution parameters
12.	Assign the modeling object to the solution.	Edit the solution to assign the rotor dynamics solution parameters modeling object to the solution.When editing the solution, you can optionally specify structural damping.	Assign a modeling object to a solution or solution subcase
13.	Define mass imbalance.	Use the Unbalance Mass command to define the loads that result from eccentric masses.Apply the loads to nodes along the axis of rotation at the location of the mass imbalances.	Create an unbalance mass
14.	Specify real modal reduction parameters.	(Optional) To perform the harmonic response solution on a reduced system, create a Real Eigenvalue modeling object to specify parameters for the real modal reduction.	Create a modeling objectAssign a modeling object to a solution or solution subcase
15.	Assign the modeling object to the subcase.	(Optional) Edit the frequency response subcase. In the Solution Step dialog box, specify modal as the solution scheme and then assign the real eigenvalue modeling object to the subcase.	Create a modeling objectAssign a modeling object to a solution or solution subcase
16.	Specify DOF for results reporting.	Use the Report command to simplify obtaining XY plots of displacement, velocity, or acceleration results for DOF of interest.	Displaying graphs in the Solution Monitor using the Report simulation object
17.	Solve the rotor dynamics model.	The Solution Monitor contains information about the status of your solution.	Solve the modelSolution Monitor
18.	Post-process the results.	Use the post-processing commands to view the harmonic response results.	Post-processing

Rotor dynamic synchronous harmonic response analysis workflow (SOL 414,111), 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 } });