Rotor dynamic analysis (SOL 414)

You can use Pre/Post to create rotor dynamic models for Simcenter Nastran SOL 414 and post-process the rotor dynamic analysis results. With Pre/Post you can create models to perform the following types of rotor dynamic analysis:

• Maneuver load analysis (SOL 414,101)Accounts for gyroscopic forces in a linear static analysisProduces results for plotting stresses, bearing forces, and damping forces

• Eigenvalues and superelement reduction analysis (SOL 414,103)Provides options for two analyses:The eigenvalue analysis computes the modes while the rotor is at rest. Use the eigenvalue analysis to validate that the model works before you add the rotations. Solving with the eigenvalue analysis is not required for generating a superelement.The superelement reduction analysis reduces a rotating part (such as a rotor defined by the Rotor Modeling Assembly simulation object) to a representation of the rotating part using the boundary nodes of the original rotating part. It condenses the rotating part to a superelement, represented by its stiffness, damping, mass, and gyroscopic matrices on selected retained nodes. For more information, see Rotor dynamic analysis with superelements (SOL 414,103).

• Complex modal analysis (SOL 414,110)Evaluates dynamic behavior of the rotating system over a range of rotor speedsProduces results for plotting Campbell diagrams and damping plots, visualizing mode shapes, and identifying critical speedsSupports direct calculation of complex modes for the entire system or the system after a real modal reductionSupports direct computation of critical speedsThe solver calculates complex eigenfrequencies for each rotation speed:ALPHA is the real part of the eigenfrequencyOMEGA is the Imaginary part of the eigenfrequencyThus, you have:Eigenfrequency = OMEGA/2PILoss Factor = -2*ALPHA/OMEGADamping = ALPHA/2PIReal part = ALPHAImaginary part = OMEGAWhirl direction = 2/forward, 3/backward, 4/linearCritical speed = intersection between eigenfrequency and velocity lines xP, where x is the order.

• Harmonic (frequency response) analysis (SOL 414,111)Accounts for frequency-dependent loadingSupports direct and modal solutionsAllows for mass imbalance of the rotorAllows for linear and nonlinear bearing propertiesProduces complex displacement, velocity, acceleration, element force, and stress results for the steady-state response in the frequency domain

• Transient response analysis (SOL 414,129)Accounts for time-dependent loadingSupports direct solution onlyAllows for linear and nonlinear bearing propertiesProduces results in the time domainAllows for inertia and damping to be disabled.

As a best practice, use the pre- and post-processing capabilities that support Simcenter Nastran SOL 414, rather than the legacy rotor dynamics capability. Some of the advantages SOL 414 rotor dynamic analysis has over the legacy rotor dynamics capabilities are as follows:

• SOL 414 contains built-in models of certain types of rolling-element bearings, squeeze-film bearings, and hydrodynamic bearings. In these models, you specify physical dimensions and material properties, and the software computes the corresponding mechanical properties. You can also model bearing rupture when you use CBUSH2 elements as bearing supports.

• SOL 414 simplifies the modeling of bearings by not requiring extra nodes that the software uses only for matrix partitioning.

• SOL 414,129 transient response analysis supports nonlinear behavior.

• SOL 414,111 allows for nonlinear bearing properties.

• SOL 414,103 allows the retained nodes to be collinear.

When you solve the model, Pre/Post writes a Simcenter Nastran SOL 414 input file. For a complete listing of the case control commands, parameters, and bulk entries that are supported for use in SOL 414, see SOL 414 Rotor Dynamics User's Guide.

The workflow to perform a SOL 414 rotor dynamic analysis is only slightly different from the workflow to perform a standard linear static analysis, complex modal analysis, harmonic analysis, or transient response analysis. The primary differences are related to creating bearing supports and specifying rotor speeds.

For analysis-specific workflow information, see the following:

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

• Rotor dynamic superelement analysis workflow (SOL 414,103)

• Rotor dynamic complex modal analysis workflow (SOL 414,110)

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

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

• Rotor dynamic transient response analysis workflow (SOL 414,129)

General modeling considerations

Static preload

For maneuver load, complex modal, and harmonic analyses, you can include static preload in your model by defining static subcases that precede the rotor dynamic subcase. For complex modal and harmonic analyses, you are limited to a single static subcase. For a maneuver load analysis, you can use multiple static subcases.

Constraints

Single-point constraints, multi-point constraints, and enforced displacements are supported.

Note:

For SOL 414,111 harmonic response analysis, when you use an enforced displacement in the frequency response subcase, you must also include a constraint for the node at which the enforced displacement is applied in the same subcase. This requirement does not exist for the other SOL 414 rotor dynamic analysis solutions, or a static subcase in a SOL 414,111 solution.

Contact

Contact is currently not supported.

Glue

Glue is supported for use in all SOL 414 analysis types.

Superelements

Simcenter Nastran superelements are supported for condensing both the non-rotating portion and the rotating parts of a SOL 414 model. For more information, see Rotor dynamic analysis with superelements (SOL 414,103).

Axisymmetry

Axisymmetry is supported for use in all SOL 414 analysis types. For more information, see Modeling axisymmetry.

Cyclic symmetry

Cyclic symmetry is supported for use in all SOL 414 analysis types except SOL 414,111 harmonic response analysis and SOL 414,103 superelement analysis. For more information, see Modeling cyclic symmetry.

Solver

The sparse solver is the solver for all SOL 414 analysis types.

Modeling rotors

You can use 1D, 2D, and 3D elements to model rotors.

You can define up to 10 rotors in a model. The rotors can be oriented differently and have different angular velocities.

To facilitate creating bearing supports, create a distinct mesh for each rotor. In these meshes, make sure that nodes are located on the axis of rotation of the rotor where bearings are located.

When Pre/Post writes the Simcenter Nastran input file, the nodes associated with the FE mesh of each rotor are written to a ROTORG bulk entry.

Modeling bearings

Unlike with the legacy rotor dynamics capability, you do not need to define extra nodes that Simcenter Nastran uses exclusively to partition matrices. Thus, it is sufficient to define a pair of coincident nodes, one of which is part of the rotor mesh and the other of which is attached to ground or the stationary portion of the model using a rigid element. You define the connectivity of the bearing elements with each pair of coincident nodes.

The primary options for modeling bearing supports are as follows:

• CBEAR2 elementsWhen you model bearing supports with CBEAR2 elements, you can define the mechanical properties explicitly, or you can define the physical dimensions and properties of built-in bearing models and let the software compute the mechanical properties. You can select from the following built-in bearing models:Rolling-element bearingsSqueeze-film bearingsHydrodynamic bearings

• CBEAR elementsWhen you model bearing supports with CBEAR elements, you explicitly define their mechanical properties.

• CBUSH elementsWhen you model bearing supports with CBUSH elements, you explicitly define their mechanical properties.

• CBUSH2 elementsWhen you model bearing supports with CBUSH2 elements, you explicitly define their mechanical properties.

Each option allows you to model the mechanical properties as speed-dependent.

Note:

If you specify that the rotor dynamic analysis is performed in a rotating reference frame, you must specify the mechanical properties of the bearings as isotropic. That is, the stiffness, damping, and mass distribution of the bearing cannot vary in the plane normal to the axis of rotation.

You can add the bearings using 1D connections or using universal connections. For more information, see Creating connection elements on a rotor model (SOL 414).

Modeling bearing rupture

CBUSH2 elements allow you to model bearing rupture. The software uses the ellipsoid criterion to predict the onset of rupture.

When the CBUSH2 element is defined as an axial bushing, the ellipsoid criterion is given as follows:

DDEN = {\left( {\frac{{{F_x}}}{{{\rm{FRUX}}}}} \right)^2} + {\left( {\frac{{{F_y}}}{{{\rm{FRUY}}}}} \right)^2} + {\left( {\frac{{{F_z}}}{{{\rm{FRUZ}}}}} \right)^2} + {\left( {\frac{{{M_x}}}{{{\rm{MRUX}}}}} \right)^2} + {\left( {\frac{{{M_y}}}{{{\rm{MRUY}}}}} \right)^2}

When the CBUSH2 element is defined as a radial bushing, the ellipsoid criterion is given as follows:

DDEN = \left( {\frac{{F_x^2 + F_y^2}}{{{\rm{FRU}}{{\rm{R}}^2}}}} \right) + {\left( {\frac{{{F_z}}}{{{\rm{FRUZ}}}}} \right)^2} + \left( {\frac{{M_x^2 + M_y^2}}{{{\rm{MRU}}{{\rm{R}}^2}}}} \right) + {\left( {\frac{{{M_z}}}{{{\rm{MRUZ}}}}} \right)^2}

where DDEN is the threshold at which rupture of the bushing is predicted to initiate, and FRUX, FRUY, FRUZ, FRUR, MRUX, MRUY, MRUZ, and MRUR are the rupture limit forces and moments of the bushing relative to a single load.

For example, FRUX is the force at which rupture initiates when the bushing is loaded by a force in the X-direction only.

If any of the FRUX, FRUY, FRUZ, FRUR, MRUX, MRUY, MRUZ, or MRUR values are not defined, the software sets the value of the quotient that contains the missing value to zero when it evaluates the ellipsoid criterion.

After the threshold value for the ellipsoid criterion has been reached, the software sets the static damage, ds, to unity. The software then uses the following relation to calculate the true damage:

\dot d = \frac{1}{{{\tau c}}}\left( {1 - {e^{ - {a_c}{{\left( {{d^s} - d} \right)} + }}}} \right)

where τc is the time parameter for delay and ac is the parameter for delay.

You specify the rupture limit forces and moments, threshold value, time parameter for delay, and parameter for delay in the PBUSH2 dialog box, on the Properties page, in the Rupture with Damage group.

Specifying rotor speeds for SOL 414,101 maneuvers analysis

To specify the rotor speeds for a SOL 414,101 maneuvers analysis, in the Rotor Dynamics Solution Parameters dialog box, set Rotation Speed Variation to Constant and enter a value in the Starting Speed (RSTART) box. In the Rotor Region dialog box, set Rotation Speed Definition to Multiplier and enter a value in the Speed Multiplier box. The software calculates the speed of a rotor to be the product of the starting speed value and the speed multiplier value for the rotor.

Specifying rotor speeds for SOL 414,110 complex modal analysis

When you perform a SOL 414,110 complex modal analysis, you can calculate the critical speeds directly, or you can create a Campbell diagram to identify the critical speeds.

To specify the rotor speeds when you calculate the critical speeds directly, in the Rotor Dynamics Solution Parameters dialog box, set Rotation Speed Variation to Linear by Steps, set Number of Steps (NUMSTEP) to zero, and enter values for Starting Speed (RSTART) and Step Size (RSTEP), even though the software does not use these values.

In the Rotor Region dialog box, set Rotation Speed Definition to Multiplier and enter a value in the Speed Multiplier box.

For a Campbell diagram, you have two options to specify the rotor speeds:

• In the Rotor Dynamics Solution Parameters dialog box, set Rotation Speed Variation to Linear by Steps and enter values in the Starting Speed (RSTART), Step Size (RSTEP), and Number of Steps (NUMSTEP) boxes to define the rotation speed range of a reference rotor.In the Rotor Region dialog box, set Rotation Speed Definition to Multiplier and enter a value in the Speed Multiplier box. The software calculates the speed of a rotor to be the product of the starting speed and the speed multiplier.

• In the Rotor Dynamics Solution Parameters dialog box, set Rotation Speed Variation to Function of Sweeping Parameter. Then create a Rotation Speeds modeling object to define a sweeping parameter for the rotational speed and assign it to the complex modal subcase. In the Rotor Region dialog box, you have two options:Set Rotation Speed Definition to Multiplier and enter a value in the Speed Multiplier box. The software calculates the speed of a rotor to be the product of the rotation speed sweeping parameter and the speed multiplier value for the rotor.Set Rotation Speed Definition to Independent and reference a function of the rotation speed sweeping parameter, which the software uses as the rotor speed.

Specifying rotor speeds for synchronous SOL 414,111 harmonic response analysis

When you perform a synchronous SOL 414,111 harmonic response analysis, you have the following options to specify the rotor speeds:

• In the Rotor Dynamics Solution Parameters dialog box, set Rotation Speed Variation to Linear by Steps, and enter values in the Starting Speed (RSTART), Step Size (RSTEP), and Number of Steps (NUMSTEP) boxes to define the speed of a reference rotor.In the Rotor Region dialog box, set Rotation Speed Definition to Multiplier and enter a value in the Speed Multiplier box. The software calculates the speed of a rotor to be the product of the reference rotor speed and the speed multiplier. The software obtains the excitation frequencies from the reference rotor speeds.For this option, in the Rotor Dynamics Solution Parameters dialog box, from the Analysis Type (SYNC) list, select Synchronous.

• In the Rotor Dynamics Solution Parameters dialog box, set Rotation Speed Variation to Function of Sweeping Parameter and create a Forcing Frequencies modeling object to define a sweeping parameter for the excitation frequencies.In the Rotor Region dialog box, set Rotation Speed Definition to Multiplier and enter 1 in the Speed Multiplier box. The software calculates the rotor speeds from the excitation frequencies.For this option, you do not need to specify Synchronous from the Analysis Type (SYNC) list.

Specifying rotor speeds and excitation frequencies for asynchronous SOL 414,111 harmonic response analysis

When you perform an asynchronous SOL 414,111 harmonic response analysis, you have the following options to specify the rotor speeds:

• In the Rotor Dynamics Solution Parameters dialog box, set Rotation Speed Variation to Constant and specify a value in the Starting Speed (RSTART) box. Create a Forcing Frequencies modeling object to define a sweeping parameter for the excitation frequencies.In the Rotor Region dialog box, set Rotation Speed Definition to Multiplier and enter a value in the Speed Multiplier box. The software calculates the speed of a rotor to be the product of the starting speed and the speed multiplier for the rotor.

• In the Rotor Dynamics Solution Parameters dialog box, set Rotation Speed Variation to Function of Sweeping Parameter and create a Forcing Frequencies modeling object to define a sweeping parameter for the excitation frequencies.In the Rotor Region dialog box, set Rotation Speed Definition to Independent and reference a function of the excitation frequency sweeping parameter, which the software uses to obtain the rotor speeds.

Specifying rotor speeds for SOL 414,129 transient response analysis

When you perform a SOL 414,129 transient response analysis, you have the following options to specify the rotor speeds:

• In the Rotor Dynamics Solution Parameters dialog box, set Rotation Speed Variation to Linear by Steps, and specify values in the Starting Speed (RSTART), Step Size (RSTEP), and Number of Steps (NUMSTEP) boxes to define the speed of a reference rotor as a linear ramp.In the Rotor Region dialog box, set Rotation Speed Definition to Multiplier and enter a value in the Speed Multiplier box. The software calculates the speed of a rotor to be the product of the reference rotor speed and the speed multiplier for the rotor.

• In the Rotor Dynamics Solution Parameters dialog box, set Rotation Speed Variation to Function of Sweeping Parameter.In the Rotor Region dialog box, set Rotation Speed Definition to Independent and reference a function that relates rotor speed and time.

Energy balance output

When solving SOL 414,110 complex modal analysis or SOL 414,111 harmonic response analysis problems, you can request that the software writes energy balance results for selected elements to the .f06 file and an external .csv file.

When you request the energy balance output, you must specify the groups of elements for which to output the results. Thus, prior to requesting the energy balance output, create groups that contain the elements of interest.

To request energy balance output, in the Rotor Dynamics Output Requests dialog box, on the Strain/Kinetic Energy Tabulation page, select the Enable SEKETAB Request check box.

For a complete listing of all the results types that you can output, see SOL 414 Rotor Dynamics User's Guide.

Modeling damping

Damping is supported for all SOL 414 solution types except maneuver load analysis (SOL 414,101). You can define viscous damping, proportional viscous damping, and hysteretic damping. When you define multiple sources of damping, the software sums the contributions from each source. For all SOL 414 solutions, you set the damping on the Parameters page in the Solution dialog box.

When you perform a SOL 414,129 transient response analysis, you can optionally disable inertia and damping. To do so, in the Nonlinear Control Parameters – Subcase dialog box, on the Analysis Control page, from the Include Inertia Effects for Nonlinear Dynamics Subcases (Inertia) list, select an option.

When you perform a SOL 414,103 eigenvalue and superelement reduction analysis, you can set Rayleigh damping for stiffness and mass, as well as overall structural damping and element structural damping. However, you can omit damping when you generate the superelement and instead apply damping on the FE Model Component Representation dialog box when you replace a component FEM file with the rotor superelement.

For more information, see Damping (SOL 414).

Symmetry and reference frames

You can perform the rotor dynamic analysis with respect to a fixed or a rotating reference frame subject to the following symmetry restrictions:

Symmetry condition	Reference frame
Symmetric rotors and supports	Fixed and rotating reference frames
Symmetric rotors and unsymmetric supports	Fixed reference frame only
Unsymmetric rotors and symmetric supports	Rotating reference frame only
Unsymmetric rotors and supports	Currently unsupported

Rotor dynamics theory is based on the axisymmetry of rotors, and different equations of motion are solved depending on whether the referenced frame is fixed or rotating.

Fixed reference frames

For axisymmetric rotors, the frame must be fixed, but the stator can be axisymmetric or symmetric. If the rotor contains concentrated masses, you must check the inertia values in mesh-associated data to ensure that:

• For CONM1 elements:Mass 44 = Mass 55

• For CONM2 elements:Mass Moment of Inertia, Ixx = Mass Moment of Inertia, Iyy****Mass Moment of Inertia, Izz = 2*Mass Moment of Inertia, Ixx

Rotating reference frames

You can select a rotating frame for any rotor geometry—the rotor can be axisymmetric or symmetric. However, for a rotating frame, the stator must be axisymmetric, and bearings must be isotropic.

When you select a rotating frame:

• The rotor is not treated as rotating.

• Unbalance loads are treated as static loads.

Therefore, for Static Loads subcases, you must take centrifugal loads (Rotation loads) into account. The Rotation load must be defined on the rotor axis, in the direction of the rotor axis, and with Angular Velocity set to 1 rad/s.

Post-processing rotor dynamic results

After Simcenter Nastran completes the solve, you can use standard post-processing capabilities to examine results from maneuver load, complex modal, harmonic, and transient response rotor dynamic analyses.

You can use a Campbell diagram to examine results from a complex modal rotor dynamic analysis. You can create a Campbell diagram directly from the Post Processing navigator or from the Scenario Based Data-Visualization Navigator. For more information, see Plot a Campbell diagram.

Where do I find it?

Application	Pre/Post
Prerequisites	A Simulation file as the work part and displayed partSimcenter Nastran as the specified solverRotor Dynamics as the specified analysis type
Command Finder	Solution

How do I

Create connection elements between coincident nodes with CBEAR2 elements

Define rotor bearing or bushing properties

Create a rotor region

Define a rotor

Define the rotor dynamics solution parameters

Create an unbalance mass

Define forcing frequencies

Define nonlinear transient parameters

Set the duration of the simulation

Create a modeling object

Assign a modeling object to a solution or solution subcase

Learn more

Modeling axisymmetry (SOL 414)

Modeling cyclic symmetry (SOL 414)

Creating connection elements on a rotor model (SOL 414)

Damping (SOL 414)

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Rotor dynamic analysis (SOL 414), 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 } });