Rotor dynamic maneuver load analysis workflow (SOL 414,101)

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 filesMaterial typesBoundary conditions
2.	Specify the Simcenter Nastran solution.	In the Solution dialog box, set the solution type to SOL 414,101 Maneuvers.	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 bearings are located.	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 how the rotor speed varies in the simulation—in a rotation speed range, or driven by the sweeping parameter of the solution and function defined in rotor region. Specify a reference frame, rotating or fixed.Note: For SOL 414,101, the software calculates the speed of a rotor to be the product of the starting speed and the speed multiplier value for the rotor.	Define the rotor dynamics solution parametersFixed reference frames and Rotating reference frames in Rotor dynamic analysis (SOL 414)
12.	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
13.	Define the angular motion.	Use the Rotation command to specify the angular velocity and angular acceleration that the model is undergoing.Note: You are limited to a single Rotation command in a subcase. Thus, to consider other states of angular motion, create additional static subcases.	RotationDefine a rotation load
14.	Solve the rotor dynamics model.	The Solution Monitor contains information about the status of your solution.	Solve the modelSolution Monitor
15.	Post-process the results.	Use the post-processing commands to view the rotor dynamics analysis results.	Post-processing

Rotor dynamic maneuver load analysis workflow (SOL 414,101), 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 } });