Chapter 14: Using Sliding Meshes

This tutorial is divided into the following sections:

14.1. Introduction

The analysis of turbomachinery often involves the examination of the transient effects due to flow interaction between the stationary components and the rotating blades. In this tutorial, the sliding mesh capability of Ansys Fluent is used to analyze the transient flow in an axial compressor stage. The rotor-stator interaction is modeled by allowing the mesh associated with the rotor blade row to rotate relative to the stationary mesh associated with the stator blade row.

For turbomachinery applications, it is recommended that connecting rotating and stationary zones utilizes General Turbo Interfaces (GTI) which can handle any pitch-change model. To know more about GTI interfaces see tutorial Modeling Blade Row Interaction using Steady-State and Transient Simulations in the Fluent Tutorials. This tutorial will show an alternative way of connecting rotating and stationary zones (using periodic repeat interface). While this tutorial is using a turbomachinery application the outlined procedure can be used for other flow applications that require the connection of similar-pitch rotating and stationary zones.

This tutorial demonstrates how to do the following:

Create periodic zones.
Set up the transient solver and cell zone and boundary conditions for a sliding mesh simulation.
Set up the mesh interfaces for a periodic sliding mesh model.
Sample the time-dependent data and view the mean value.

14.2. Prerequisites

This tutorial is written with the assumption that you have completed the introductory tutorials found in this manual and that you are familiar with the Ansys Fluent outline view and ribbon structure. Some steps in the setup and solution procedure will not be shown explicitly.

14.3. Problem Description

The model represents a single-stage axial compressor composed of two blade rows. The first row is the rotor with 16 blades, which is operating at a rotational speed of 37,500 rpm. The second row is the stator with 32 blades. The blade counts are such that the domain is rotationally periodic, with a periodic angle of 22.5 degrees. This enables you to model only a portion of the geometry, namely, one rotor blade and two stator blades. Due to the high Reynolds number of the flow and the relative coarseness of the mesh (both blade rows are composed of only 13,856 cells total), the analysis will employ the inviscid model, so that Ansys Fluent is solving the Euler equations.

Figure 14.1: Rotor-Stator Problem Description

14.4. Setup and Solution

The following sections describe the setup and solution steps for this tutorial:

14.4.1. Preparation

To prepare for running this tutorial:

Download the sliding_mesh.zip file here .
Unzip sliding_mesh.zip to your working directory.
The mesh file axial_comp.msh.h5 can be found in the folder.
Use the Fluent Launcher to start Ansys Fluent.
Select Solution in the top-left selection list to start Fluent in Solution Mode.
Select 3D under Dimension.
Enable Double Precision under Options.
Set Solver Processes to 1 under Parallel (Local Machine).

14.4.2. Mesh

Read in the mesh file axial_comp.msh.h5.
File → Read → Mesh...

14.4.3. General Settings

Check the mesh.
Domain → Mesh → Check → Perform Mesh Check
Ansys Fluent will perform various checks on the mesh and will report the progress in the console. Ensure that the reported minimum volume is a positive number.
Warnings will be displayed regarding unassigned interface zones, resulting in the failure of the mesh check. You do not need to take any action at this point, as this issue will be rectified when you define the mesh interfaces in a later step.
Examine the mesh (Figure 14.2: Rotor-Stator Display).
Orient the view to display the mesh as shown in Figure 14.2: Rotor-Stator Display. The inlet of the rotor mesh is colored blue, the interface between the rotor and stator meshes is colored yellow, and the outlet of the stator mesh is colored red.
Figure 14.2: Rotor-Stator Display
Define the units for the model.
Setup → General → Units...
1. Select angular-velocity from the Quantities selection list.
2. Select rev/min from the Units selection list.
3. Select pressure from the Quantities selection list.
  Scroll down the Quantities list to find pressure.
4. Select atm from the Units selection list.
5. Close the Set Units dialog box.
Change zones rotor-per-1 and rotor-per-3 from wall zones to periodic zones.
Setup → Boundary Conditions → Wall
1. Click rotor-per-1 to select the tree item.
2. While holding down the Ctrl key, click rotor-per-3 to add the tree item to the selection.
  Note: The first zone that is selected will be used as the periodic zone, while the second zone will be used as the shadow zone. Although it is not significant in this case, the order in which the two zone pairs are selected may affect simulation results.
3. Right-click the selected tree items and select Periodic... to open the Create Periodic dialog box.
4. Select Rotational in the Type group box.
5. Click Create to close the Create Periodic dialog box.
Similarly, change the following wall zone pairs to periodic zones:
Zone Pairs Respective Zone IDs
rotor-per-2 and rotor-per-4 12 and 11
stator-per-1 and stator-per-3 26 and 27
stator-per-2 and stator-per-4 24 and 25

Zone Pairs	Respective Zone IDs
`rotor-per-2` and `rotor-per-4`	`12` and `11`
`stator-per-1` and `stator-per-3`	`26` and `27`
`stator-per-2` and `stator-per-4`	`24` and `25`

14.4.4. Models

Enable the inviscid model.
Setup → Models → Viscous Edit...
1. Select Inviscid in the Model list.
2. Click OK to close the Viscous Model dialog box.

14.4.5. Materials

Specify air (the default material) as the fluid material, using the ideal gas law to compute density.
Setup → Materials → Fluid → air Edit...
1. Retain the default entry of air in the Name text entry field.
2. Select ideal-gas from the Density drop-down list in the Properties group box.
3. Retain the default values for all other properties.
4. Click Change/Create and close the Create/Edit Materials dialog box.
As reported in the console, Ansys Fluent will automatically enable the energy equation, since this is required when using the ideal gas law to compute the density of the fluid.
Specify that it is a transient problem, to allow mesh motion.
Setup → General
1. Retain the default selection of Pressure-Based in the Type list.
2. Select Transient in the Time list.

14.4.6. Cell Zone Conditions

Setup → Cell Zone Conditions

Set the cell zone conditions for the fluid in the rotor (fluid-rotor).
Setup → Cell Zone Conditions → fluid-rotor → Edit...
1. Enable Mesh Motion.
2. Click the Mesh Motion tab.
3. Retain the default values of (0, 0, 1) for X, Y, and Z in the Rotation-Axis Direction group box.
4. Enter 37500 rpm for Speed in the Rotational Velocity group box.
5. Click Apply and close the Fluid dialog box.
Set the cell zone conditions for the fluid in the stator (fluid-stator).
Setup → Cell Zone Conditions → fluid-stator → Edit...
1. Retain the default values of (0, 0, 1) for X, Y, and Z in the Rotation-Axis Direction group box.
2. Click Apply and close the Fluid dialog box.

14.4.7. Boundary Conditions

Setup the rotor-inlet boundary condition.
Setup → Boundary Conditions → Inlet → rotor-inlet → Edit...
1. Enter 1.0 atm for Gauge Total Pressure.
2. Enter 0.9 atm for Supersonic/Initial Gauge Pressure.
  For information about the Supersonic/Initial Gauge Pressure, see the Fluent User's Guide.
3. Click the Thermal tab and enter 288 K for Total Temperature.
4. Click Apply and close the Pressure Inlet dialog box.
Enter stator-outlet into the Zone field to filter the zone list.
Setup → Boundary Conditions → Outlet → stator-outlet → Edit...
1. Enter 1.08 atm for Gauge Pressure.
2. Enable Radial Equilibrium Pressure Distribution.
3. Click the Thermal tab and enter 288 K for Backflow Total Temperature.
4. Click Apply and close the Pressure Outlet dialog box.
Note: The momentum settings and temperature you input at the pressure outlet will be used only if flow enters the domain through this boundary. It is important to set reasonable values for these downstream scalar values, in case flow reversal occurs at some point during the calculation.
Retain the default boundary conditions for all wall zones.
Setup → Boundary Conditions → Wall → rotor-blade-1 → Edit...
Note: For wall zones, Ansys Fluent always imposes zero velocity for the normal velocity component, which is required whether or not the fluid zone is moving. This condition is all that is required for an inviscid flow, as the tangential velocity is computed as part of the solution.

14.4.8. Operating Conditions

Set the operating pressure.
Setup → Boundary Conditions → Operating Conditions...
1. Enter 0 atm for Operating Pressure.
2. Click OK to close the Operating Conditions dialog box.
Since you have specified the boundary condition inputs for pressure in terms of absolute pressures, you have to set the operating pressure to zero. Boundary condition inputs for pressure should always be relative to the value used for operating pressure.

14.4.9. Mesh Interfaces

Disable the one-to-one interface creation method using the following text command, so that you can create a mesh interface that uses the Periodic Repeats option.
```
define/mesh-interfaces/one-to-one-pairing? no
```
Create a periodic mesh interface between the rotor and stator mesh regions.
1. Open the Mesh Interfaces dialog box.
  Setup → Mesh Interfaces New...
2. Click Manual Create... to open the Create/Edit Mesh Interfaces dialog box.
3. Enter int for Mesh Interface.
4. Enable Periodic Repeats in the Interface Options group box.
  Enabling this option, allows Ansys Fluent to treat the interface between the sliding and non-sliding zones as periodic where the two zones do not overlap.
5. Select rotor-interface from the Interface Zones Side 1 selection list.
  Note: In general, when one interface zone is smaller than the other, it is recommended that you choose the smaller zone as Interface Zone 1. In this case, since both zones are approximately the same size, the order is not significant.
6. Select stator-interface from the Interface Zones Side 2 selection list.
7. Click Create/Edit... and close the Create/Edit Mesh Interfaces dialog box.
8. Close the Mesh Interfaces dialog box.
Check the mesh again to verify that the warnings displayed earlier have been resolved.
Domain → Mesh → Perform Mesh Check

14.4.10. Solution

Set the solution parameters.
Solution → Solution → Methods...
Select Coupled from the Pressure-Velocity Coupling group box.
Change the Solution Controls
Solution → Controls → Controls...
1. Enter 0.5 for Momentum and Pressure in the Explicit Relaxation Factors group box.
2. Enter 0.9 for Temperature in the Under-Relaxation Factors group box.
Enable the plotting of residuals during the calculation.
Solution → Reports → Residuals...
1. Ensure that the Plot is selected in the Options group box.
2. Enable Show Advanced Options and select relative from the Convergence Criterion drop-down list.
3. Enter 0.01 for Relative Criteria for each Residual (continuity, x-velocity, y-velocity, z-velocity, and energy).
4. Click OK to close the Residual Monitors dialog box.
Enable the plotting of mass flow rate at the inlet (rotor-inlet).
Solution → Reports → Definitions → New → Surface Report → Mass Flow Rate...
1. Enter surf-mon-1 for the Name of the surface report definition.
2. In the Create group box, enable Report File, Report Plot and Print to Console.
3. Enter rotor-inlet in the Surfaces field to filter the list.
4. Select rotor-inlet from the Surfaces selection list.
5. Click OK to save the surface report definition settings and close the Surface Report Definition dialog box.
  surf-mon-1-rplot and surf-mon-1-rfile that are automatically generated by Fluent appear in the tree (under Solution/Monitors/Report Plots and Solution/Monitors/Report Files, respectively).
Enable the plotting of mass flow rate at the outlet (stator-outlet).
Solution → Reports → Definitions → New → Surface Report → Mass Flow Rate...
1. Enter surf-mon-2 for the Name of the surface report definition.
2. In the Create group box, enable Report File, Report Plot and Print to Console.
3. Enter stator-outlet in the Surfaces field to filter the list.
4. Select stator-outlet from the Surfaces selection list.
5. Click OK to save the surface report definition settings and close the Surface Report Definition dialog box.
  surf-mon-2-rplot and surf-mon-2-rfile that are automatically generated by Fluent appear in the tree (under Solution/Monitors/Report Plots and Solution/Monitors/Report Files, respectively).
Enable the plotting of the area-weighted average of the static pressure at the interface (stator-interface).
Solution → Reports → Definitions → New → Surface Report → Area-Weighted Average...
1. Enter surf-mon-3 for the Name of the surface report definition.
2. In the Create group box, enable Report File, Report Plot and Print to Console.
3. Retain the default selection of Pressure... and Static Pressure from the Field Variable drop-down lists.
4. Enter stator-interface in the Surfaces field to filter the list.
5. Select stator-interface from the Surfaces selection list.
6. Click OK to save the surface report definition settings and close the Surface Report Definition dialog box.
  surf-mon-3-rplot and surf-mon-3-rfile that are automatically generated by Fluent appear in the tree (under Solution/Monitors/Report Plots and Solution/Monitors/Report Files, respectively).
Initialize the solution using the values at the inlet (rotor-inlet).
Solution → Initialization → Options...
1. Select rotor-inlet from the Compute from drop-down list.
2. Select Absolute in the Reference Frame list.
3. Click Initialize.
Save the initial case file (axial_comp.cas.h5).
File → Write → Case...
Run the calculation for one revolution of the rotor.
Solution → Run Calculation → Run Calculation...
1. Enter 6.6667e-6 s for Time Step Size.
  The time step is set such that the passing of a single rotor blade is divided into 15 time steps. There are 16 blades on the rotor. Therefore, in each time step the rotor rotates 360/16/15=1.5 degrees. With a rotational speed of 37,500 rpm (225,000 deg/sec), 1.5 degrees of rotation takes 1.5 / 2.25e5 = 6.6667e-6 sec.
2. Enter 240 for Number of Time Steps.
  There are 16 blades on the rotor, and each rotor blade period corresponds to 15 time steps (see above). Therefore, a complete revolution of the rotor will take 16*15=240 time steps.
3. Retain the default setting of 20 for Max Iterations/Time Step.
4. Click Calculate.
The residuals jump at the beginning of each time step and then fall at least two to three orders of magnitude. Also, the relative convergence criteria is achieved before reaching the maximum iteration limit (20) for each time step, indicating the limit does not need to be increased.
Figure 14.3: Residual History for the First Revolution of the Rotor
Examine the flow variable histories for the first revolution of the rotor (Figure 14.4: Mass Flow Rate at the Inlet During the First Revolution, Figure 14.5: Mass Flow Rate at the Outlet During the First Revolution, and Figure 14.6: Static Pressure at the Interface During the First Revolution).
Figure 14.4: Mass Flow Rate at the Inlet During the First Revolution

Figure 14.5: Mass Flow Rate at the Outlet During the First Revolution

Figure 14.6: Static Pressure at the Interface During the First Revolution

The flow variable histories show that the large variations in flow rate and interface pressure that occur early in the calculation are greatly reduced as time-periodicity is approached.
Save the case and data files (axial_comp-0240.cas.h5 and axial_comp-0240.dat.h5).
File → Write → Case & Data...
Note: It is a good practice to save the case file whenever you are saving the data file especially for sliding mesh model. This is because the case file contains the mesh information, which is changing with time.
Note: For transient-state calculations, you can add the character string %t to the file name so that the iteration number is automatically appended to the name (for example, by entering axial_comp-%t for the File Name in the Select File dialog box, Ansys Fluent will save files with the names axial_comp-0240.cas.h5 and axial_comp-0240.dat.h5).
Rename the report output file in preparation for further iterations.
Solution → Monitors → Report Files → surf-mon-1-rfile Edit...
1. Enter surf-mon-1b.out for Output File Base Name.
2. Click OK to close the Edit Report File dialog box.
Similarly, change the output file names for the surf-mon-2-rfile and surf-mon-3-rfile report file definitions to surf-mon-2b.out and surf-mon-3b.out, respectively.
Continue the calculation for 720 more time steps to simulate three more revolutions of the rotor.
Solution → Run Calculation → Run Calculation...
Examine the flow variable histories for the next three revolutions of the rotor to verify that the solution is time-periodic (Figure 14.7: Mass Flow Rate at the Inlet During the Next 3 Revolutions Figure 14.8: Mass Flow Rate at the Outlet During the Next 3 Revolutions, and Figure 14.9: Static Pressure at the Interface During the Next 3 Revolutions).
Figure 14.7: Mass Flow Rate at the Inlet During the Next 3 Revolutions

Figure 14.8: Mass Flow Rate at the Outlet During the Next 3 Revolutions

Figure 14.9: Static Pressure at the Interface During the Next 3 Revolutions
Save the case and data files (axial_comp-960.cas.h5 and axial_comp-960.dat.h5).
File → Write → Case & Data...
Change the file names for surf-mon-1b.out, surf-mon-2b.out, and surf-mon-3b.out to surf-mon-1c.out, surf-mon-2c.out, and surf-mon-3c.out, respectively (as described in a previous step), in preparation for further iterations.
Add a point at the interface of the stator.
Results → Surface → Create → Point...
1. Enter -0.02 for x, -0.08 for y, and -0.036 for z in the Point Surface dialog box.
2. Enter point-1 for Name.
3. Click Create and close the Point Surface dialog box.
Enable plotting of the static pressure at a point on the stator interface (point-1).
Solution → Reports → Definitions → New → Surface Report → Vertex Average...
1. Enter surf-mon-4 for the Name of the surface report definition.
2. In the Create group box, enable Report File, Report Plot and Print to Console.
3. Retain the defaults of Pressure and Static Pressure for Field Variable.
4. Enter point-1 in the Surfaces field to filter the list.
5. Select point-1 from the Surfaces selection list.
6. Click OK to save the surface report definition settings and close the Surface Report Definition dialog box.
Continue the calculation for one final revolution of the rotor, while saving data samples for the postprocessing of the time statistics.
Solution → Run Calculation → Run Calculation...
1. Enter 240 for Number of Time Steps.
2. Enable Data Sampling for Time Statistics in the Options group box.
  Enabling Data Sampling for Time Statistics causes Ansys Fluent to calculate and store mean and root-mean-square (RMS) values of various quantities and field functions over the calculation interval.
3. Click Calculate.
Save the case and data files (axial_comp-1200.cas.h5 and axial_comp-1200.dat.h5).
File → Write → Case & Data...
Figure 14.10: Static Pressure at a Point on The Stator Interface During the Final Revolution

14.4.11. Postprocessing

Examine the vertex-averaged static pressure at the stator during the final revolution of the rotor (as calculated from surf-mon-4.out), and plot the data.
Results → Plots → FFT...
1. Click the Load Input File... button to open the Select File dialog box.
  1. Select All Files from the Files of type: drop-down list.
  2. Select surf-mon-4-rfile.out from the list of files.
  3. Click OK to close the Select File dialog box.
2. Click the Plot/Modify Input Signal... button to open the Plot/Modify Input Signal dialog box.
  1. Enable Subtract Mean Value in the Options group box.
  2. Enter flow-time as the X Axis Label.
  3. Select flow-time in the X Axis Variable drop-down list.
  4. Click Apply/Plot.
  5. Close the Plot/Modify Input Signal dialog box.
3. Click Plot FFT in the Fourier Transform dialog box.
4. Click Axes... to open the Axes - Fourier Transform dialog box.
5. Select exponential from the Type drop-down list, and set Precision to 1 in the Number Format group box.
6. Click Apply and close the Axes - Fourier Transform dialog box.
7. Click Plot FFT and close the Fourier Transform dialog box.
Figure 14.11: FFT of Static Pressure at the Stator

The FFT plot clearly shows that the pressure fluctuations due to interaction at the interface are dominated by the rotor and stator blade passing frequencies (which are 10 kHz and 20 kHz, respectively) and their higher harmonics.
Display contours of the mean static pressure on the walls of the axial compressor.
Results → Graphics → Contours → New...
1. Enter contour-mean-static-pressure for Contour Name.
2. Ensure Filled is enabled in the Options group box.
3. Select Banded in the Coloring group box.
4. Select Unsteady Statistics... and Mean Static Pressure from the Contours of drop-down lists.
5. Select Wall from the Surface Types selection list.
  Scroll down the Surfaces selection list to find Wall.
6. Click Save/Display and close the Contours dialog box.
7. Rotate the view to get the display as shown in Figure 14.12: Mean Static Pressure on the Outer Shroud of the Axial Compressor.
Shock waves are clearly visible in the flow near the outlets of the rotor and stator, as seen in the areas of rapid pressure change on the outer shroud of the axial compressor.
Figure 14.12: Mean Static Pressure on the Outer Shroud of the Axial Compressor
Save the case file (axial_comp-1200.cas.h5).
File → Write → Case...

14.5. Summary

This tutorial has demonstrated the use of the sliding mesh model for analyzing transient rotor-stator interaction in an axial compressor stage. The model utilized the coupled pressure-based solver in conjunction with the transient algorithm to compute the inviscid flow through the compressor stage. The solution was calculated over time until the reported variables displayed time-periodicity (which required several revolutions of the rotor), after which time-averaged data was collected while running the case for the equivalent of one additional rotor revolution (240 time steps).

The Fast Fourier Transform (FFT) utility in Ansys Fluent was employed to determine the time averages from stored flow variable report data. You also used the FFT utility to examine the frequency content of the transient report data. The observed peak corresponds to the passing frequency and the higher harmonics of the passing frequency, which occurred at approximately 10,000 Hz.