This tutorial includes:
Important: This tutorial requires file TimeBladeRowIni_001.res, which is produced by following tutorial Time Transformation Method for a Transient Rotor-stator Case.
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 | |
|
CCL File |
Import | |
|
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) | ||
|
Domain Interface |
Fluid Solid | |
|
Domain Solver Control |
Timescale Factor | |
|
CFX-Solver Manager |
Derived Variable |
Average solid temperature |
|
CFD-Post |
Plots |
Contour |
|
Data Instancing | ||
|
Time Chart |
This tutorial sets up a transient blade row calculation with conjugate heat transfer using the Time Transformation model. It uses an axial turbine to illustrate the basic concepts of setting up, running, and monitoring a transient blade row problem with conjugate heat transfer in Ansys CFX. It also describes the postprocessing of transient blade row and conjugate heat transfer results using the tools provided in CFD-Post for this type of calculation.
The full geometry of the axial rotor-stator stage selected for modeling contains 36 stator blades and 42 rotor blades.
The geometry to be modeled consists of a single rotor blade passage, a single stator blade passage, and a single solid rotor blade. Each rotor blade passage is an 8.571° section (360°/42 blades), while each stator blade passage is a 10° section (360°/36 blades). The pitch ratio at the interface between the rotor passage and the stator passage is 0.8571 (that is, 6/7).
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 rotor-stator geometry, a 1/6 machine section (7 rotor blades, 6 stator blades) would produce a pitch ratio of 1.0, but this would require a model about 7 times larger than in this tutorial example.
In this example, the rotor rotates about the Z axis at 3500 rev/min (positive rotation following the right hand rule) while the stator is 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. These profiles were obtained from previous simulations of the upstream and downstream stages. In this tutorial, a separate total temperature profile is applied to the stator inlet via CEL expressions that are provided in a .ccl file. This profile is of total temperature in a Gaussian distribution with a maximum that is 50% higher than the baseline value.
In this tutorial, conjugate heat transfer is modeled between the rotor blade passage and the solid rotor blade. The solid rotor blade domain is defined and the conjugate heat transfer interface is created. The timescale factor setting is adjusted in the domain solver control settings for the solid rotor blade to accelerate the solid thermal diffusion convergence.
The following steps outline the overall approach:
Define the transient blade row simulation using the Turbomachinery wizard in CFX-Pre.
Import the stator and rotor meshes, which were created in Ansys TurboGrid.
Enter the basic model definition.
Import the solid blade mesh, which was created in ICEM CFD.
Set the profile boundary conditions using CFX-Pre in General mode.
Create a fluid-solid interface to model conjugate heat transfer between the rotor blade passage and the solid rotor blade
Set the timescale factor in domain solver control for the solid rotor blade.
Run the transient blade row simulation using the steady-state results from Time Transformation Method for a Transient Rotor-stator Case as an initial guess.
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.
Download the
time_blade_row_cht.zipfile here .Unzip
time_blade_row_cht.zipto your working directory.Ensure that the following tutorial input files are in your working directory:
TBRCHTCEL.cclTBRInletProfile.csvTBROutletProfile.csvTBRTurbineRotor.gtmTBRTurbineSolid.cfx5TBRTurbineStator.gtmTimeBladeRowIni_001.res(produced by following tutorial Time Transformation Method for a Transient Rotor-stator Case)
Set the working directory and start CFX-Pre.
For details, see Setting the Working Directory and Starting Ansys CFX in Stand-alone Mode.
This tutorial uses the Turbomachinery wizard in CFX-Pre. This preprocessing mode is designed to simplify the setup of turbomachinery simulations.
In CFX-Pre, select > .
Select Turbomachinery and click .
Select > .
Under File name, type
TimeBladeRowCHT.Click .
If you are notified that the file already exists, click .
In the Basic Settings panel, configure the following settings:
Setting
Value
Machine Type
Axial Turbine
Axes
> Coordinate Frame
Coord 0
Axes
> Rotation Axis
Z
Analysis Type
> Type
Transient Blade Row
Analysis Type
> Method
Time Transformation
Click .
You will define two new components and import their respective meshes.
Right-click in the blank area and select Add Component from the shortcut menu.
Create a new component of type
StationarynamedS1and click .Configure the following setting(s):
Setting
Value
Mesh
> File
TBRTurbineStator.gtm [ a ]
Create a new component of type
Rotating, namedR1and click .Configure the following setting(s):
Setting
Value
Component Type
> Value
3500 [rev min^-1] [ a ]
Mesh
> File
TBRTurbineRotor.gtm
Click .
In this section you will set properties of the fluid domain and some solver parameters.
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
Transient Rotor Stator
Continue to click until you reach
Final Operations.Set Operation to
Enter General Modebecause you will continue to define the simulation through settings not available in the Turbomachinery wizard.Click .
Verify the following settings, which affect the accuracy of the simulation:
Edit
R1.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)
Click .
In the Outline tree view, right-click
Meshand select Import Mesh > ICEM CFD.The Import Mesh dialog box appears.
Configure the following setting(s):
Setting
Value
File name
TBRTurbineSolid.cfx5
Options
> Mesh Units
m[ a ]
Click Open.
In this section you will define the solid domain for the blade and initialize the domain temperature to a reasonable value. You will also adjust the Timescale Factor setting in the solver control options. This setting is used in transient cases involving conjugate heat transfer to increase the thermal response of the solid. This is done to compensate for the large disparity in time scales between fluid convection and solid diffusion, which makes transient modeling of such problems otherwise impractical. The initialization and solver control options that are set when creating a domain apply only to that domain.
Rename
Default DomaintoRotor Solid Blade.Edit
Rotor Solid Blade.Configure the following setting(s):
Tab
Setting
Value
Basic Settings
Location and Type
> Domain Type
Solid Domain
Solid Definitions
> Solid 1
> Material
Aluminum [ a ]
Domain Models
> Domain Models
> Option
Rotating
Domain Models
> Domain Motion
> Angular Velocity
3500 [rev min^-1]
Domain Models
> Passage Definition
> Pass. in Component
1
Domain Models
> Passage Definition
> Passages in 360
42
Initialization
Domain Initialization
(Selected)
Domain Initialization
> Initial Conditions
> Temperature
> Option
Automatic with Value
Domain Initialization
> Initial Conditions
> Temperature
> Temperature
300 [K]
Solver Control
Domain Solver Control
(Selected)
Domain Solver Control
> Timescale Control
> Timescale Factor
1.0e6[ b ]
The timescale factor is defined as: solid time scale /
, where 
is the simulation time-step size necessary to resolve
flow features of interest. Increasing the timescale factor to 1.0e6
from the default 1 increases the physical time scale of this transient
run inside the solid domain by a factor of 1.0e6.
Click .
The inlet and outlet boundary conditions are defined using profiles in your working directory and several CEL expressions. Boundary profile data must be initialized before they can be used for boundary conditions.
Select Tools > Initialize Profile Data.
The Initialize Profile Data dialog box appears.
Beside Profile Data File, click Browse
.The Select Profile Data File dialog box appears.
From your working directory, select
TBRInletProfile.csv.Click .
Click .
The profile data is read into memory.
Under Data File, click Browse
.From your working directory, select
TBROutletProfile.csv.Click .
Click .
Select File > Import > CCL.
Ensure that Import Method is set to Append.
Select
TBRCHTCEL.ccl.Click .
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.
Edit
S1 Inlet.Configure the following setting(s):
Tab
Setting
Value
Basic Settings
Profile Boundary Conditions
> Use Profile Data
(Selected)
Profile Boundary Setup
> Profile Name
inlet
Click .
This causes the profile values of
Total PressureandTotal Temperatureto 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.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
TINLET
Click .
Edit
R1 Outlet.Configure the following setting(s):
Tab
Setting
Value
Basic Settings
Frame Type
Rotating
Profile Boundary Conditions
> Use Profile Data
(Selected)
Profile Boundary Setup
> Profile Name
outlet
Click Generate Values.
Configure the following setting(s):
Tab
Setting
Value
Boundary Details
Mass And Momentum
> Option
Static Pressure
Mass and Momentum
> Relative Pressure
outlet.Pressure(r)
Click .
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.
Edit
S1 InletConfigure the following setting(s):
Tab
Setting
Value
Plot Options
Boundary Contour
(Selected)
Profile Variable
Total Temperature
Click Apply
CFX-Pre plots the Total Pressure radial profile at the inlet with the pressure values displayed in a legend.
Here you will edit the
default boundary in Rotor Solid Blade to create
the hub boundary for the blade.
Rename
Rotor Solid Blade DefaulttoBlade Base.Edit
Blade Base.On the Basic Settings tab, set Location to
Hub 2.On the Boundary Details tab, ensure that Heat Transfer > Option is set to
Adiabatic.Click .
Click Insert > Domain Interface and, in the dialog box that appears, set Name to
CHT Interfaceand click .Configure the following setting(s) of
CHT Interface:Click .
An error message related to the domain
R1will appear in the message window. This error occurs because the 2D RegionBLADE 2inR1is being used in both a boundary and a domain interface. This error is resolved in the next step.Delete the boundary
R1 Bladein the domainR1.
You will set the simulation to be solved using the Time Transformation method.
Edit
Transient Blade Row Models.Configure the following setting(s):
Setting
Value
Transient Method
> Time Period
> Option
Passing Period
Transient Method
> Time Period
> Domain
S1
Transient Method
> Time Steps
> Option
Number of Timesteps per Period
Transient Method
> Time Steps
> Timesteps/Period
35
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 as: 2 * pi / (Passages in 360 * Signal 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 to be used for postprocessing.
The time step size is also automatically calculated as: Passing Period / Number of Timesteps per Period. The Timestep setting cannot be edited.
Click .
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. You will also add the Wall
Heat Flux variable to the default list to observe the results
of the conjugate heat transfer.
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:
Click Output Control
.Click the Trn Results tab.
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, Wall Heat Flux[ a ]
Click the Monitor tab.
Configure the following setting(s):
Setting
Value
Monitor Objects
(Selected)
Monitor Objects
> Efficiency Output
(Cleared)
Create a monitor point named
rotor_P1.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]
Create an additional monitor point named
stator_P1.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]
Create an additional monitor point named
solid_P1.Under Monitor Objects > Monitor Points and Expressions > solid_P1, configure the following settings:
Setting
Value
Option
Cylindrical Coordinates
Output Variables List
Temperature
Position Axial Comp.
0.224 [m]
Position Radial Comp.
0.2755 [m]
Position Theta Comp.
181 [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, three monitor points will be used for demonstration purposes.
Click .
Click Define Run
.Configure the following setting(s):
Setting
Value
File name
TimeBladeRowCHT.def
Click .
Ignore the error message (the initial values for
R1andS1will be specified in CFX-Solver Manager) and click to continue.CFX-Solver Manager automatically starts and, on the Define Run dialog box, Solver Input File is set.
If using stand-alone mode, quit CFX-Pre, saving the simulation (
.cfx) file at your discretion.
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.
Ensure that the Define Run dialog box is displayed. If an error message appears, ignore it and click to continue.
Solver Input File should be set to
TimeBladeRowCHT.def.Under the Initial Values tab, select Initial Values Specification.
Under Initial Values Specification > Initial Values, select
Initial Values 1.Under Initial Values Specification > Initial Values > Initial Values 1 Settings > File Name, click Browse
.Select
TimeBladeRowIni_001.resfrom your working directory.Click Open.
Under Initial Values Specification > Use Mesh From, select
Solver Input File.Click .
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.
After the simulation has proceeded for some time, observe the periodic nature of the monitor point values.
While the solver is running, create and then monitor a derived variable for the average solid temperature over the last period:
Open the New Derived Variable dialog box in any of these ways:
Select Workspace > New Derived Variable.
Select Workspace > Workspace Properties.
The Workspace Properties dialog box appears.
Select the Derived Variables tab.
Click New
.Right-click in the chart area and select Monitor Properties from the context menu.
The Monitor Properties dialog box appears.
Select the Derived Variables tab.
Click New
.
Set Name to
Moving Averageand click OK.The Derived Variable Properties dialog box appears.
Set Statistics > Statistics Type to
Arithmetic Average.Ensure that the settings specify that the average is over a moving interval of one time period, then click OK.
The derived variable is created.
Click OK to dismiss the Workspace Properties dialog box, if applicable.
In the Monitor Properties dialog box (right-click in the chart area and select Monitor Properties from the context menu), select the Plot Lines tab.
Expand the tree to
USER POINT>Temperature>solid_P1, then right-clicksolid_P1and select Add Derived Plot Line For Variable > Moving Average.Click OK to dismiss the Monitor Properties dialog box.
After at least one interval has passed, observe that the User Points tab shows a plot for
solid_P1 (Temperature), Moving Average.
When CFX-Solver is finished, select the check box next to Post-Process Results.
Click .
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:
Start CFD-Post and load
TimeBladeRowCHT_001.res.When CFD-Post opens, if you see the Domain Selector dialog box, ensure that all the domains are selected, then click to load the results from these domains.
If you see a message regarding transient blade row postprocessing, click .
Click Timestep Selector
.Select the 1st time step.
Click to load the time step, and then click Close to exit the dialog box.
The rotor blades move to their starting positions.
Create a plane to be used for making plots:
Select Insert > Location > Plane. Accept the default name and click .
Configure the following setting(s):
Tab
Setting
Value
Geometry
Domains
Rotor Solid Blade
Definition
> Method
ZX Plane
Definition
> Y
-0.27 [m]
Click .
Turn off the visibility of
Plane 1by clearing its check box in the Outline tree view.
Click Insert > Contour and accept the default name.
Configure the following setting(s):
Tab
Setting
Value
Geometry
Locations
Plane 1
Variable
Temperature.Trnavg[ a ]
Range
Local
# of Contours
31
Click .
The contour plot shows
Temperaturevalues corresponding to arithmetic averages calculated using the results from all time steps.
In this section, you will compute and plot the magnitude of the heat flow 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 35 time steps per stator blade passing period and there are six stator blade passing periods in a common period. Therefore, the total number of intermediate time steps in the common period is 210. For this case, the solver has reconstructed results over two common periods (420 time steps). You will reduce the total number of time steps to 140 to speed up the generation of the time chart.
Reduce the number of time steps in the period:
Click Timestep Selector
.Configure the following setting(s):
Tab
Setting
Value
Timestep Selector
Timestep Sampling
Uniform
Number of Timesteps
70
Click .
The Timestep Selector now shows a total of 140 steps over two common periods (shown under the Phase column).
Compute the heat flow on the blade:
Select Insert > Expression.
In the Insert Expression dialog box, type
heat flow on solid blade.Click .
Set Definition, to
areaInt(Wall Heat Flux)@CHT Interface Side 1Click to create the expression.
Create a transient chart showing heat flow:
Select Insert > Chart and accept the default name.
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
heat flow on solid blade
Click .
A chart showing heat flow on a single rotor blade against time is created, added to the chart object, and displayed in the Chart Viewer.
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.
From the Outline tree view, edit
Contour 1.In the Geometry tab, set Location to
CHT Interface Side 1.Click .
From the Outline tree view, edit
Rotor Solid Blade.In the Data Instancing tab, set Number of Data Instances to 7.
Click .
Turn off the visibility of
Wireframe.
On the 3D Viewer tab, CFD-Post displays the group of rotor blades corresponding to 1/6 of a full wheel (the minimum number of blades that makes a unity pitch ratio between stator and rotor passages).
The data-dependent transient heat flow on solid blade on Chart 1 is still showing the result computed
on a single solid blade. After you expand the number of solid rotor
blades to 7, the CHT Interface Side
1 groups all 7 rotor blades together and the total heat
flow should be updated. To update the chart, click the Refresh button at the top of the Chart Viewer.
The heat flow on solid blade expression
is now being computed on all 7 solid rotor blades.