OS-T: 1372 Rotor Dynamics of a Hollow Cylindrical Rotor

In this tutorial you will perform Rotor Dynamics analysis on a hollow cylindrical rotor.

Before you begin, copy the file(s) used in this tutorial to your working directory.

For rotating components, additional forces like the gyroscopic force and circular damping force exist and are critical in the study of their response. It is important to determine these effects of rotating components on the system as a whole. Here the complex eigenvalue analysis for 0, 10K, 30K, and 50K RPM are run.

The objective is to determine critical frequencies, and generate Campbell diagram when subjected to a static imbalance from the rotor. At the critical frequency you observe forward/backward cylindrical and conical whirl (mode shapes).

os_1372_model
Figure 1. Model Review
rotor.fem File Data
  • 1D Line Mesh is created using beam elements for the Rotor
  • Rotor is defined with Material MAT1
  • Rotor is defined with Beam Property
  • SPC condition is defined in the model

    os_1372_bar
    Figure 2.

Launch HyperMesh and Set the OptiStruct User Profile

  1. Launch HyperMesh.
    The User Profile dialog opens.
  2. Select OptiStruct and click OK.
    This loads the user profile. It includes the appropriate template, macro menu, and import reader, paring down the functionality of HyperMesh to what is relevant for generating models for OptiStruct.

Import the Model

  1. Click File > Import > Solver Deck.
    An Import tab is added to your tab menu.
  2. For the File type, select OptiStruct.
  3. Select the Files icon files_panel.
    A Select OptiStruct file browser opens.
  4. Select the rotor.fem file you saved to your working directory.
  5. Click Open.
  6. Click Import, then click Close to close the Import tab.

Set Up the Model

Create EIGRL and EIGC Cards

In this step, a modal method is used to solve the complex eigenvalue problem, which is more computationally efficient compared to extracting the complex modes directly. With this approach, first, the real modes are calculated via a normal modes analysis. Then, a complex eigenvalue problem is formed on the projected subspace spanned by the real modes which is much smaller than the real space. Here, both EIGRL and EIGC cards need to be defined.
  1. In the Model Browser, right-click and select Create > Load Step Inputs.
  2. In the Name field, enter EIGRL.
  3. For Config type, select Real Eigen Value Extraction.
  4. For Type, select EIGRL from the drop-down menu.
  5. Click V2 and input 250.0.
    250.0 is defined as the highest frequency bond.
  6. Create another load step input named EIGC.
  7. For Config type, select Complex Eigen Value Extraction.
  8. For Type, verify the default EIGC is selected.
  9. Click NORM and select MAX.
    MAX option is used to normalize the eigenvectors.
  10. For ND0 OPTIONS, select User Defined from the drop-down menu.
  11. Click ND0 and input 55.
    The desired number of roots to be extracted is 55.

Define Grids for the Rotor Line Model

  1. Right-click in the Model Browser and select Create > SET.
  2. Click Name and enter ROTORG_SET.
  3. Click Card Image and select ROTORG from the drop-down menu.
  4. Click Entity IDs and click on nodes.
  5. Select nodes by collector and select CBEAM, and proceed.
  6. Check the box next to the RSPINR field since every rotor defined via ROTORG requires a corresponding RSPINR entry.
  7. Click the field next to GRIDA and then Node.
  8. In the selection panel, click Node and enter 10000 in the ID= field.
  9. Similarly, for GRIDB, enter 10001.
  10. Click on the field next to SPTID and enter 1.0.

Create RSPEED Load Collector

  1. In the Model Browser, right-click and select Create > Load Collector.
  2. Click Name and enter RSPEED.
  3. Click Card Image and select RSPEED from the drop-down menu.
  4. Click S1 and enter 0.0, which is first reference rotor speed.
  5. Click DS and enter 10000.0, which is increment in reference rotor speed.
  6. Click NDS and enter 5, which is the number of reference rotor speed increments.

Create RGYRO Load Step Inputs

  1. In the Model Browser, right-click and select Create > Load Step Inputs.
  2. Click Name and enter RGYRO.
  3. Click Config type and select Rotordynamic Analysis Parameters from the drop-down menu.
  4. For Type, verify RGYRO is selected.
  5. Click SYNCFLG and select ASYNC from the drop-down menu.
    Tip: This is set to run an Asynchronous Rotor dynamics analysis.
  6. Click REFROTR and click set.
  7. Select ROTORG_SET and click OK.
  8. Check the field next to SPEED_ID.
  9. Next to the SPEED field, click Unspecified > Loadcol and select RSPEED from the pop-up window.

Define Load Step for Modal Complex Eigenvalue Analysis

  1. In the Model Browser, right-click and select Create > Load Step.
  2. In the Name field, enter Rotor Dynamics.
  3. Click Analysis type and select Complex eigen (modal) from the drop-down menu.
  4. For SPC, select SPC from the list of load collectors.
  5. For CMETHOD, select EIGC from the list of load step inputs.
  6. For METHOD(STRUCT), select EIGRL from the list of load step inputs.
  7. Under SUBCASE OPTIONS, check the field next to RGYRO and then RGYRO_ID.
  8. Click on the field next to ID to select load step input RGYRO.

Submit the Job

  1. From the Analysis page, click the OptiStruct panel.

    OS_1000_13_17
    Figure 3. Accessing the OptiStruct Panel
  2. Click save as.
  3. In the Save As dialog, specify location to write the OptiStruct model file and enter rotor_async for filename.
    For OptiStruct input decks, .fem is the recommended extension.
  4. Click Save.
    The input file field displays the filename and location specified in the Save As dialog.
  5. Set the export options toggle to all.
  6. Set the run options toggle to analysis.
  7. Set the memory options toggle to memory default.
  8. Click OptiStruct to launch the OptiStruct job.
If the job is successful, new results files should be in the directory where the rotor_async.fem was written. The rotor_async.out file is a good place to look for error messages that could help debug the input deck if any errors are present.

Run the Model

  1. Click on the RGYRO card in the Model Browser.
  2. Click SYNCFLG and change from ASYNC to SYNC from the drop-down menu.

  1. From the Analysis page, enter the OptiStruct panel.
  2. Click Save as following the input file: field.
    A Save As browser window opens.
  3. Select the directory where you would like to write the file and enter the name rotor_sync.fem in the File name: field.
  4. Click Save.
    Note: The name and location of the file displays in the input file: field.
  5. Set the export options: toggle to all.
  6. Set the run options: toggle to Analysis.
  7. Set the memory options: toggle to memory default.
  8. Click OptiStruct. This launches the OptiStruct job.

If the job completed successfully, new results files can be seen in the directory where the OptiStruct model file was written. The rotor_sync.out file is a good place to look for error messages that will help to debug the input deck if any errors are present.

View the Results

Complex eigenvalue analysis computes the complex modes of the structure. The eigenvalues of the complex modes can be found in rotor_async.out file. The complex eigenvectors can be reviewed in HyperView.
  1. Read the rotor_async.out in HyperView.To get the Campbell Diagram and review the critical frequencies at the intersection points, select Campbell Diagram Instructions.

    os_1372_campbell_diagram
    Figure 4.
    TableView in HyperView provides a summary for the critical frequencies.

    os_1372_tableview_summary
    Figure 5.
  2. Load the rotor_sync.out file in a text editor.
    The Frequencies which you get from the Synchronous Rotor dynamic analysis give you the critical frequencies. The complex modes contain the imaginary part, which represents the cyclic frequency, and the real part which represents the damping of the mode. If the real part is negative, then the mode is said to be stable. If the real part is positive, then the mode is unstable.

    os_1372_text_editor
    Figure 6. Eigenvalues of the Complex Modes
  3. Compare to verify the Critical Frequencies which you obtained from the intersection points and the frequencies you obtained in the rotor_sync.out file.
  4. Load the rotor_async.h3d file into HyperView to review and verify below Cylindrical and Conical mode shapes.
    RPM Cylindrical Modes Forward

    Mode #3

    		 Cylindrical Modes Backward

    Mode #4

    		 Conical Modes Forward

    Mode #5

    		 Conical Modes Backward

    Mode #6
    10,000 2.802E+00 2.802E+00 1.248E+01 1.248E
    30,000 2.802E+00 2.802E+00 1.201E+01 1.201E+01
    50,000 2.802E+00 2.802E+00 1.058E+01 1.058E+1