Chapter 37: Time Transformation Method for a 1.5-stage Transient Rotor-stator Case

This tutorial includes:

 

37.1. Tutorial Features

In this tutorial you will learn about:

Component

Feature

Details

CFX-Pre

User Mode

Turbo Wizard

General mode

Analysis Type

Transient Blade Row

Fluid Type

Air Ideal Gas

Domain Type

Multiple Domains

Rotating Frame of Reference

Turbulence Model

Shear Stress Transport

Heat Transfer

Total Energy

Boundary Conditions

Inlet (Subsonic)

Outlet (Subsonic)

Wall (Counter Rotating)

CFD-Post

Plots

Vector

Contour

Data Instancing

Time Chart

Animation

 

37.2. Overview of the Problem to Solve

This tutorial sets up a 1.5-stage transient blade row calculation using the Time Transformation model. It uses a 1.5-stage machine to illustrate the basic concepts of setting up, running, and monitoring a transient blade row problem in Ansys CFX. It also describes the postprocessing of multistage transient blade row results using the tools provided in CFD-Post for this type of calculation.

The full geometry of the 1.5 stages selected for modeling contains 36 blades in the first stator row, 42 blades in the rotor row, and 37 blades in the second stator row.

The geometry to be modeled consists of a single rotor blade passage and two stator blade passages (one from each stator row). Each rotor blade passage is an 8.571° section (360°/42 blades), while the blade passages from the first stator row are 10° sections (360°/36 blades) and the blade passages from the second stator row are 9.730° sections (360°/37 blades). The pitch ratio at the interface between the rotor passage and the first stator passage is 0.8571 (that is, 6/7). The pitch ratio at the interface between the rotor passage and the second stator passage is 0.8810 (that is, 37/42).

For the Time Transformation method, you should always maintain an ensemble pitch ratio within a range of 0.75 to 1.4. Note that the range of permissible pitch ratios narrows significantly with slower rotation speed. A full machine analysis can be performed (modeling all rotor and stator blades), which always eliminates any pitch change, but will require significant computational time. For this geometry, only a full machine analysis can produce a pitch ratio of 1.0.

In this example, the rotor rotates about the Z axis at 3500 rev/min (positive rotation following the right hand rule) while the stator rows are stationary. Rotational periodicity boundaries are used to enable only a small section of the full geometry to be modeled.

The flow is modeled as being turbulent and compressible. Profile boundary conditions are used at the inlet and outlet. In this tutorial, the profiles are a function of the radial coordinate only. These profiles were obtained from previous simulations of the upstream and downstream stages.

The overall approach of this tutorial is to run a transient blade row simulation initialized with the results of a steady-state simulation. First, you will define a steady-state simulation using the Turbomachinery Wizard followed by General mode. While the steady-state simulation is running, you will modify a copy of it to define a transient blade row simulation that uses the Time Transformation model. After running the transient blade row simulation, you will create contour plots and an animation showing blade rotation.

If this is the first tutorial you are working with, it is important to review the following topics before beginning:

 

37.3. Preparing the Working Directory

  1. Create a working directory.

    Ansys CFX uses a working directory as the default location for loading and saving files for a particular session or project.

  2. Download the m_time_blade_row.zip file here .

  3. Unzip m_time_blade_row.zip to your working directory.

    Ensure that the following tutorial input files are in your working directory:

    • TBRInletProfile.csv

    • TBROutlet2Profile.csv

    • TBRTurbineRotor.gtm

    • TBRTurbineStator.gtm

    • TBRTurbineStator2.gtm

  4. Set the working directory and start CFX-Pre.

    For details, see Setting the Working Directory and Starting Ansys CFX in Stand-alone Mode.

 

37.4. Defining a Steady-state Case in CFX-Pre

This tutorial uses the Turbomachinery wizard in CFX-Pre. This preprocessing mode is designed to simplify the setup of turbomachinery simulations.

  1. In CFX-Pre, select File > New Case.

  2. Select Turbomachinery and click OK.

  3. Select File > Save Case As.

  4. Under File name, type MTimeBladeRowIni.

  5. Click Save.

  6. If you are notified that the file already exists, click Overwrite.

 

37.4.1. Basic Settings

  1. In the Basic Settings panel, configure the following settings:

    Setting

    Value

    Machine Type

    Axial Turbine

    Axes

    > Rotation Axis

     

    Z

    Analysis Type

    > Type

     

    Steady State

  2. Leave the other settings at their default values.

  3. Click Next.

 

37.4.2. Components Definition

You will define three new components and import their respective meshes.

  1. Right-click in the blank area and select Add Component from the shortcut menu.

  2. Create a new component of type Stationary named S1 and click OK.

  3. Configure the following setting(s):

    Setting

    Value

    Mesh

    > File

     

    TBRTurbineStator.gtm [a]

    1. You may have to select the CFX Mesh (*gtm *cfx) option under Files of type.

  4. Create a new component of type Rotating, named R1 and click OK.

  5. Configure the following setting(s):

    Setting

    Value

    Component Type

    > Value

     

    3500 [rev min^-1] [a]

    Mesh

    > File

     

    TBRTurbineRotor.gtm

    1. From the problem description.

  6. Create a new component of type Stationary named S2 and click OK.

  7. Configure the following setting(s):

    Setting

    Value

    Mesh

    > File

     

    TBRTurbineStator2.gtm

  8. Click Next.

 

37.4.3. Physics Definition

In this section you will set properties of the fluid domain and some solver parameters.

  1. In the Physics Definition panel, configure the following:

    Setting

    Value

    Fluid

    Air Ideal Gas

    Model Data

    > Reference Pressure

     

    0 [atm] [a]

    Model Data

    > Heat Transfer

     

    Total Energy

    Model Data

    > Turbulence

     

    Shear Stress Transport

    Inflow/Outflow Boundary Templates

    > P-Total Inlet P-Static Outlet

     

    (Selected)

    Inflow/Outflow Boundary Templates

    > Inflow

    > P-Total

     

     

    169000 [Pa][b]

    Inflow/Outflow Boundary Templates

    > Inflow

    > T-Total

     

     

    306 [K][b]

    Inflow/Outflow Boundary Templates

    > Inflow

    > Flow Direction

     

     

    Normal to Boundary

    Inflow/Outflow Boundary Templates

    > Outflow

    > P-Static

     

     

    110000 [Pa][b]

    Interface

    > Default Type

     

    Stage

    1. To define the simulation using absolute pressure, set this value to 0 atm.

    2. These values are temporary. They will be replaced with profile data later in the tutorial.

  2. Continue to click Next until you reach Final Operations.

  3. Set Operation to Enter General Mode because you will continue to define the simulation through settings not available in the Turbomachinery wizard.

  4. Click Finish.

 

37.4.4. Additional Fluid Model Settings

Verify the following settings, which affect the accuracy of the simulation:

  1. Edit R1.

  2. Configure the following setting(s):

    Tab

    Setting

    Value

    Basic Settings

    Domain Models

    > Domain Motion

    > Alternate Rotation Model

     

     

    (Selected)

    Fluid Models

    Heat Transfer

    > Incl. Viscous Work Term

     

    (Selected)

  3. Click OK.

 

37.4.5. Initializing Profile Boundary Conditions

The inlet and outlet boundary conditions are defined using profiles in your working directory. Boundary profile data must be initialized before they can be used for boundary conditions.

  1. Select Tools > Initialize Profile Data.

    The Initialize Profile Data dialog box appears.

  2. Beside Profile Data File, click Browse  .

    The Select Profile Data File dialog box appears.

  3. From your working directory, select TBRInletProfile.csv.

  4. Click Open.

  5. Click Apply.

    The profile data is read into memory.

  6. Beside Profile Data File, click Browse  .

    The Select Profile Data File dialog box appears.

  7. From your working directory, select TBROutlet2Profile.csv.

  8. Click Open.

  9. Click OK.

Note:  After profile data has been initialized from a file, the profile data file should not be deleted or otherwise removed from its directory. By default, the full filepath to the profile data file is stored in CFX-Pre, and the profile data file is read directly by CFX-Solver each time the solver is started or restarted.

 

37.4.6. Modifying Inlet and Outlet Boundary Conditions

  1. Edit S1 Inlet.

  2. Configure the following setting(s):

    Tab

    Setting

    Value

    Basic Settings

    Profile Boundary Conditions

    > Use Profile Data

     

    (Selected)

    Profile Boundary Setup

    > Profile Name

     

    inlet

  3. Click Generate Values.

    This causes the profile values of Total Pressure and Total Temperature to be applied at the nodes on the inlet boundary. It also causes entries to be made in the Boundary Details tab. In order to later reset the velocity values at the main inlet to match those that were originally read from the profile data file, revisit the Basic Settings tab for this boundary and click Generate Values.

  4. Configure the following setting(s):

    Tab

    Setting

    Value

    Boundary Details

    Mass and Momentum

    > Option

     

    Total Pressure (stable)

    Mass and Momentum

    > Relative Pressure

     

    inlet.Total Pressure(r)

    Flow Direction

    > Option

     

    Cylindrical Components

    Flow Direction

    > Axial Component

     

    1

    Flow Direction

    > Radial Component

     

    0

    Flow Direction

    > Theta Component

     

    0

    Heat Transfer

    > Total Temperature

     

    inlet.Total Temperature(r)

  5. Click OK.

  6. Edit S2 Outlet.

  7. Configure the following setting(s):

    Tab

    Setting

    Value

    Basic Settings

    Profile Boundary Conditions

    > Use Profile Data

     

    (Selected)

    Profile Boundary Setup

    > Profile Name

     

    outlet

  8. Click Generate Values.

  9. Configure the following setting(s):

    Tab

    Setting

    Value

    Boundary Details

    Mass And Momentum

    > Option

     

    Static Pressure

    Mass and Momentum

    > Relative Pressure

     

    outlet.Pressure(r)

  10. Click OK.

 

37.4.7. Visualizing the Profile Boundary Value

You can plot scalar profile values and vectors on inlet and outlet boundaries. In this section, you will edit a boundary so that you can visualize the pressure profile values at the inlet.

  1. Edit S1 Inlet

  2. Configure the following setting(s):

    Tab

    Setting

    Value

    Plot Options

    Boundary Contour

    (Selected)

    Profile Variable

    Relative Pressure

  3. Click Apply

CFX-Pre plots the Total Pressure radial profile at the inlet with the pressure values displayed in a legend.

 

37.4.8. Writing the CFX-Solver Input (.def) File

  1. Click Define Run  .

  2. Configure the following setting(s):

    Setting

    Value

    File name

    MTimeBladeRowIni.def

  3. Click Save.

    CFX-Solver Manager automatically starts and, on the Define Run dialog box, Solver Input File is set.

  4. Save the simulation.

 

37.5. Obtaining a Solution to the Steady-state Case

Ensure that the Define Run dialog box is displayed in CFX-Solver Manager.

  1. Click Start Run.

    CFX-Solver runs and attempts to obtain a solution. At the end of the run, a dialog box is displayed stating that the simulation has ended.

  2. Ensure that the Post-Process Results check box is cleared.

  3. Click OK.

 

37.6. Defining a Transient Blade Row Case in CFX-Pre

In the second part of the tutorial, you will modify the simulation from the first part of the tutorial to model the transient blade row.

 

37.6.1. Opening the Existing Case

This step involves opening the original simulation and saving it to a different location.

  1. Ensure that the following tutorial input files are in your working directory:

    • MTimeBladeRowIni.cfx

    • MTimeBladeRowIni_001.res

    • TBRInletProfile.csv

    • TBROutlet2Profile.csv

  2. Set the working directory and start CFX-Pre if it is not already running.

    For details, see Setting the Working Directory and Starting Ansys CFX in Stand-alone Mode.

  3. If the original simulation is not already opened, then open MTimeBladeRowIni.cfx.

  4. Save the case as MTimeBladeRow.cfx in your working directory.

 

37.6.2. Modifying the Analysis Type

In this section, you will make use of the transient blade row feature.

Modify the analysis type as follows:

  1. Edit Analysis Type.

  2. Configure the following setting(s):

    Setting

    Value

    Analysis Type

    > Option

     

    Transient Blade Row

    Analysis Type

    > Initial Time

    > Option

     

     

    Automatic with Value

    Analysis Type

    > Initial Time

    > Time

     

     

    0 [s]

  3. Click OK.

 

37.6.3. Modifying the Rotor–stator Interfaces

  1. Edit R1 to S1.

  2. Configure the following setting(s):

    Setting

    Value

    Interface Models

    > Frame Change/Mixing Model

    > Option

     

     

    Transient Rotor Stator

  3. Click OK.

  4. Edit S2 to R1.

  5. Configure the following setting(s):

    Setting

    Value

    Interface Models

    > Frame Change/Mixing Model

    > Option

     

     

    Transient Rotor Stator

  6. Click OK.

 

37.6.4. Setting up a Transient Blade Row Model

You will set the simulation to be solved using the Time Transformation method.

  1. Edit Transient Blade Row Models.

  2. Set Transient Blade Row Model > Option to Time Transformation.

  3. Under Time Transformation, click Add new item  , accept the default name, and click OK.

  4. Configure the following setting(s):

    Setting

    Value

    Transient Method

    > Time Period

    > Option

     

     

    Passing Period

    Transient Method

    > Time Period

    > Domain

     

     

    R1

    Transient Method

    > Time Steps

    > Option

     

     

    Number of Timesteps per Period

    Transient Method

    > Time Steps

    > Timesteps/Period

     

     

    60

    Transient Method

    > Time Duration

    > Option

     

     

    Number of Periods per Run

    Transient Method

    > Time Duration

    > Periods per Run

     

     

    10

    Note:

    • The passing period is automatically calculated using 2 * pi / (Number of Blades * Angular Velocity). The Passing Period setting cannot be edited.

    • The number of time steps per period should always be larger than 2 * Number of Fourier Coefficients + 1 for use during postprocessing.

    • The time step size is also automatically calculated as: Passing Period / Number of Timesteps per Period. The Timestep setting cannot be edited.

  5. Under Time Transformation, click Add new item  , accept the default name, and click OK.

  6. Configure the following setting(s):

    Setting

    Value

    Time Transformation

    > Time Transformation 2

     

    (Selected)

    Time Transformation 2

    > Domain Interface

     

    S2 to R1

  7. Click OK.

 

37.6.5. Setting Output Control and Creating Monitor Points

For transient blade row calculations, a minimal set of variables are selected to be computed using Fourier coefficients. It is convenient to postprocess variables in the stationary frame when multiple frames of reference are present. Here, you will add the Velocity in Stn Frame and Mach Number in Stn Frame variables to the default list.

In addition, monitor points can be used to effectively compare the Time Transformation results against a reference case. They provide useful information on the quality of the reference phase and frequency produced in the simulation. They should be used to monitor convergence and, as the simulation converges, the user points should display a periodic pattern.

Note:

  • When comparing to a reference case, make sure monitor points are placed in the same relative locations with respect to the initial configuration in both cases.

  • It is important to check that the solver equations are being solved correctly. Monitoring pressure provides feedback on the momentum equations while monitoring temperature provides feedback on the energy equations.

Set up the output control and create monitor points as follows:

  1. Click Output Control  .

  2. Click the Trn Results tab.

  3. Configure the following setting(s):

    Setting

    Value

    Transient Blade Row Results

    > Extra Output Variables List

     

    (Selected)

    Transient Blade Row Results

    > Extra Output Variables List

    > Extra Output Var. List

     

     

    Velocity in Stn Frame, Mach Number in Stn Frame[a]

    1. Click Multi-select from extended list   and hold down the Ctrl key while selecting each of the listed variables.

  4. Click the Monitor tab.

  5. Configure the following setting(s):

    Setting

    Value

    Monitor Objects

    (Selected)

    Monitor Objects

    > Efficiency Output

     

    (Cleared)

  6. Create a monitor point named rotor_P1.

  7. Under Monitor Objects > Monitor Points and Expressions > rotor_P1, configure the following settings:

    Setting

    Value

    Option

    Cylindrical Coordinates

    Output Variables List

    Pressure, Temperature, Total Pressure, Total Temperature, Velocity

    Position Axial Comp.

    0.211 [m]

    Position Radial Comp.

    0.2755 [m]

    Position Theta Comp.

    182 [degree]

  8. Create an additional monitor point named stator_P1.

  9. Under Monitor Objects > Monitor Points and Expressions > stator_P1, configure the following settings:

    Setting

    Value

    Option

    Cylindrical Coordinates

    Output Variables List

    Pressure, Temperature, Total Pressure, Total Temperature, Velocity

    Position Axial Comp.

    0.202 [m]

    Position Radial Comp.

    0.2755 [m]

    Position Theta Comp.

    178 [degree]

  10. Create an additional monitor point named rotor_P2.

  11. Under Monitor Objects > Monitor Points and Expressions > rotor_P2, configure the following settings:

    Setting

    Value

    Option

    Cylindrical Coordinates

    Output Variables List

    Pressure, Temperature, Total Pressure, Total Temperature, Velocity

    Position Axial Comp.

    0.27 [m]

    Position Radial Comp.

    0.2755 [m]

    Position Theta Comp.

    176 [degree]

  12. Create an additional monitor point named stator_P2.

  13. Under Monitor Objects > Monitor Points and Expressions > stator_P2, configure the following settings:

    Setting

    Value

    Option

    Cylindrical Coordinates

    Output Variables List

    Pressure, Temperature, Total Pressure, Total Temperature, Velocity

    Position Axial Comp.

    0.28 [m]

    Position Radial Comp.

    0.2755 [m]

    Position Theta Comp.

    174 [degree]

    Note:  Transient blade row cases use monitor points to monitor the periodic fluctuating variable values. For diagnostic purposes, you should have several monitor points. Here, four monitor points are used for demonstration purposes.

  14. Click OK.

 

37.6.6. Writing the CFX-Solver Input (.def) File

  1. Click Define Run  .

  2. Configure the following setting(s):

    Setting

    Value

    File name

    MTimeBladeRow.def

  3. Click Save.

  4. Ignore the error message (the initial values will be specified in CFX-Solver Manager) and click Yes to continue.

    CFX-Solver Manager automatically starts and, on the Define Run dialog box, Solver Input File is set.

  5. If using stand-alone mode, quit CFX-Pre, saving the simulation (.cfx) file at your discretion.

 

37.7. Obtaining a Solution to the Transient Blade Row Case

At this point, CFX-Pre has been shut down, and the Define Run dialog box is displayed in CFX-Solver Manager. You will now obtain a solution to the CFD problem. To reduce the simulation time, the simulation will be initialized using a steady-state case.

  1. Ensure that the Define Run dialog box is displayed. If an error message appears, ignore it and click Yes to continue.

    Solver Input File should be set to MTimeBladeRow.def.

  2. Under the Initial Values tab, select Initial Values Specification.

  3. Under Initial Values Specification > Initial Values, select Initial Values 1.

  4. Under Initial Values Specification > Initial Values > Initial Values 1 Settings > File Name, click Browse  .

  5. Select MTimeBladeRowIni_001.res from your working directory.

  6. Click Open.

  7. Under Initial Values Specification > Use Mesh From, select Solver Input File.

  8. Click Start Run.

    CFX-Solver runs and attempts to obtain a solution. At the end of the run, a dialog box is displayed stating that the simulation has ended.

    Note:

    • Before the simulation begins, the "Transient Blade Row Post-processing Information" summary in the CFX-Solver Output file will display the time step range over which the solver will accumulate the Fourier coefficients.

    • Similarly, the "Time Transformation Stability" summary in the CFX-Solver Output file displays whether the rotor-stator pitch ratio is within the acceptable range.

    • After the CFX-Solver Manager has run for a short time, you can track the monitor points you created in CFX-Pre by clicking the Time Corrected User Points tab that appears at the top of the graphical interface of CFX-Solver Manager.

    • Monitor points of similar values can be grouped together by right-clicking on any monitor tab and selecting New Monitor. Change Type to Plot Monitor and click OK. Expand USER POINT and select the points of interest (for example, all the pressure points), then click OK.

    • After the simulation has proceeded for some time, observe the periodic nature of the monitor point values.

  9. When CFX-Solver is finished, select the check box next to Post-Process Results.

  10. Click OK.

 

37.8. Viewing the Time Transformation Results in CFD-Post

In a transient blade row run, flow field variables are compressed using the Fourier coefficient method. These variables are accumulated at the end of the simulation. This enables you to navigate through any time instance, within the common period, without having to load multiple transient results files. By default CFD-Post displays results corresponding to the end the simulation.

To get started, follow these steps:

  1. Start CFD-Post and load MTimeBladeRow_001.res.

  2. When CFD-Post opens, if you see the Domain Selector dialog box, ensure that all the domains are selected, then click OK to load the results from these domains.

  3. If you see a message regarding transient blade row postprocessing, click OK.

 

37.8.1. Creating a Turbo Surface

Create a turbo surface to be used for making plots:

  1. Click the Turbo tab.

  2. If you see the Turbo Initialization dialog box, click Yes, otherwise click the Initialize All Components button, which is visible initially by default, or after double-clicking the Initialization object in the Turbo tree view.

  3. Select Insert > Location > Turbo Surface.

  4. Change the name to Span 50.

  5. Configure the following setting(s):

    Tab

    Setting

    Value

    Geometry

    Definition

    > Method

     

    Constant Span

    Definition

    > Value

     

    0.5

  6. Click Apply.

  7. Turn off the visibility of Span 50 by clearing its check box in the Outline tree view.

 

37.8.2. Creating a Vector Plot

  1. Click Insert > Vector and accept the default name.

  2. Configure the following setting(s):

    Tab

    Setting

    Value

    Geometry

    Definition

    > Locations

     

    Span 50

    Definition

    > Variable

     

    Velocity in Stn Frame

  3. Click Apply.

    The vector plot shows Velocity in Stn Frame values corresponding to the end of a common period.

    The rotor domain is in the angular position corresponding to its location after 10 passing periods. Now you will align the rotor with the stator, as it was in the solver input file.

  4. Click Timestep Selector  .

  5. Select the 1st time step.

  6. Click Apply to load the time step, and then click Close to exit the dialog box.

    The rotor blades move to their starting positions.

 

37.8.3. Creating a Blade-to-Blade Plot

  1. Turn off the visibility of Vector 1.

  2. In the Turbo tab, edit Plots > Blade-to-Blade.

  3. Configure the following setting(s):

    Setting

    Value

    Span

    0.5

    Plot Type

    Contour

    Variable

    Pressure

    Range

    Local

    # of Contours

    21

  4. Click Apply.

The contour plot shows Pressure values corresponding to the specified time step.

 

37.8.4. Creating a Chart of Force on a Rotor Blade versus Time

In this section, you will compute and plot the magnitude of the forces that the flow applies on the rotor blade. For a transient blade row case, CFD-Post automatically reconstructs variables for the flow solution time based on the last time step. Intermediate time steps for time instances in the common period are located in the Timestep Selector. In Setting up a Transient Blade Row Model, you set 60 time steps per rotor blade passing period and there are 42 rotor blade passing periods in a common period. Therefore, the total number of intermediate time steps in the common period is 2520. For this case, the solver has reconstructed results over one common period (2520 time steps). You will reduce the total number of time steps to 420 to speed up the generation of the time chart.

Reduce the number of time steps in the period:

  1. Click Timestep Selector  .

  2. Configure the following setting(s):

    Setting

    Value

    Timestep Sampling

    Uniform

    Number of Timesteps

    420

  3. Click Apply.

    The Timestep Selector now shows a total of 420 steps over one common period (shown under the Phase column).

Compute the forces on the blade:

  1. Select Insert > Expression.

  2. In the Insert Expression dialog box, type forces on rotor blade.

  3. Click OK.

  4. Set Definition to sqrt(force_x()@ R1 Blade ^2 + force_y()@ R1 Blade ^2 + force_z()@ R1 Blade ^2)

  5. Click Apply to create the expression.

Create a transient chart showing force:

  1. Select Insert > Chart and accept the default name.

  2. Configure the following setting(s):

    Tab

    Setting

    Value

    General

    XY - Transient or Sequence

    (Selected)

    Data Series

    Series 1

    > Data Source

    > Expression

     

     

    (Selected)

    Series 1

    > Data Source

    > Expression

     

     

    forces on rotor blade

  3. Click Apply.

    A chart showing the force on a single rotor blade versus time is created and displayed in the Chart Viewer.

 

37.8.5. Creating a Chart of a Solution Monitor and Fourier Coefficient Data for Pressure versus Time

In this section, you will plot a solution monitor.

First, create a chart of the pressure at monitor point stator_P1 versus time:

  1. From the main menu, select Insert > Chart.

  2. Accept the default name by clicking OK.

  3. Configure the following setting(s):

    Tab

    Setting

    Value

    General

    XY - Transient or Sequence

    (Selected)

    Data Series

    Series 1

    > Name

     

    stator_P1 Pressure Solver Data

    stator_P1 Pressure Solver Data

    > Data Source

    > Monitor Data

     

     

    (Selected)

    stator_P1 Pressure Solver Data

    > Monitor Variable Selection

    > Y Axis

    > Variable

     

     

     

    Monitor Point: stator_P1 (Pressure) [a]

    1. Click Browse Variables   to open the Monitor Data Y Variable dialog box. From the tree in the dialog box, select User Point > Pressure > stator_P1. Click OK.

  4. Click Apply.

    A chart showing the raw solver pressure data at monitor point stator_P1 versus time is created and displayed in the Chart Viewer.

Next, create another data series that will show the pressure signal reconstructed from Fourier coefficients at the same point in the stator as monitor point stator_P1.

Start by adding a point:

  1. From the main menu, select Insert > Location > Point.

  2. Accept the default name by clicking OK.

  3. Set Method to XYZ.

  4. Set Point coordinates to -0.2778, 0.01044, 0.2021.

  5. Click Apply.

    Note the location of Point 1 in the viewer.

Next, create the chart series:

  1. Edit Chart 2.

  2. In the Chart 2 details view, on the Data Series tab, click New   to add a new series.

  3. Configure the following setting(s):

    Tab

    Setting

    Value

    Data Series

    Series 2

    > Name

     

    stator_P1 Pressure Fourier Coefficients

    stator_P1 Pressure Fourier Coefficients

    > Data Source

    > Location

     

     

    Point 1

    X Axis

    Axis Range

    > Determine ranges automatically

     

    (Cleared)

    Axis Range

    > Min

     

    0

    Axis Range

    > Max

     

    0.00415405

    Y Axis

    Data Selection

    > Variable

     

    Pressure

  4. Click Apply.

    The chart now also shows the pressure at point Point 1 versus time, as represented by the Fourier coefficient data. The reconstructed pressure signal is based on Fourier coefficients and the blade passing period and is therefore an approximation of the raw solver pressure data.

 

37.8.6. Setting up Data Instancing Transformations

In this section, you will create additional copies of the original passages that replicate mesh nodes at different locations with correct space and time interpolation values. After the data instancing process, CFD-Post will create additional mesh nodes proportional to the number of extra passages created, and populate them with solution variables correctly updated to their corresponding position in time and space.

  1. From the Outline tree view, edit R1.

  2. In the Data Instancing tab, set Number of Data Instances to 42.

  3. Click Apply.

  4. From the Outline tree view, edit S1.

  5. In the Data Instancing tab, set Number of Data Instances to 36.

  6. Click Apply.

  7. From the Outline tree view, edit S2.

  8. In the Data Instancing tab, set Number of Data Instances to 37.

  9. Click Apply.

  10. Turn off the visibility of Wireframe.

On the 3D Viewer tab, CFD-Post displays the group of blades corresponding to a full wheel (the minimum number of blades that makes a unity pitch ratio between stator and rotor passages).

If you click the Turbo tab, then the 3D Viewer shows the contour plot that you made earlier. Notice that the contour plot is now expanded to include the full wheel. Notice also that the solution varies around the wheel.

The data-dependent transient forces on rotor blade on Chart 1 is still showing the result computed on a single blade passage. After you expand the number of rotor blades in the rotor passage to 42, the R1 Blade groups all 42 rotor blades together and the total force should be updated. To update the chart, click the Refresh button at the top of the Chart Viewer.

The forces on rotor blade expression is now being computed on all 42 blades in the extended number of passages in the rotor.

 

37.8.7. Animating the Movement of the Rotor Relative to the Stator

With the Timestep Selector set to time step 0, you will make an animation showing the relative motion starting from this time step and lasting for one stator blade passing period.

  1. Click the 3D Viewer tab.

  2. Position the geometry for the animation by right-clicking on a blank area in the viewer and selecting Predefined Camera > View From -X.

  3. Click Animation  .

    The Animation dialog box appears.

  4. Set Type to Keyframe Animation.

  5. Click New   to create KeyframeNo1.

  6. Select KeyframeNo1, then set # of Frames to 70, then press Enter while in the # of Frames box.

    Tip:  Be sure to press Enter and confirm that the new number appears in the list before continuing.

    This will place 70 intermediate frames between the keyframes, for a total of 72 frames.

  7. Use the Timestep Selector to load time step 70 and then close the dialog box.

  8. In the Animation dialog box, click New to create KeyframeNo2.

  9. Click More Animation Options   to expand the Animation dialog box.

  10. Select Save Movie.

  11. Specify a filename for the movie.

  12. Set Format to MPEG1.

  13. Click To Beginning   to rewind the active keyframe to KeyframeNo1.

    Note:  The active keyframe is indicated by the value appearing in the F: field in the middle of the Animation dialog box. In this case it will be 1.

    Wait for CFD-Post to finish loading the objects for this frame before proceeding.

  14. Click Save animation state   and save the animation to a file. This will enable you to quickly restore the animation in case you want to make changes. Animations are not restored by loading ordinary state files (those with the .cst extension).

  15. Click Play the animation  .

    Note:  It takes a while for the animation to be completed. To view the movie file, you will need to use a media player that supports the MPEG format.

    From the animation and plots, you can see that the flow is continuous across the interface. This is because CFD-Post is capable of interpolating the flow field variables to the correct time and position using the computed Fourier coefficients.

  16. When you have finished, close the Animation dialog box and then close CFD-Post, saving the animation state at your discretion.