Fill out the form to download

Required field
Required field
Not a valid email address
Required field
Required field
  • Set up your own cloud-native simulation in minutes.

  • Documentation

    Advanced Tutorial: Fluid Flow Simulation Through a Water Turbine

    This tutorial showcases how to use SimScale to run an incompressible fluid simulation on a water turbine using rotating zones. The complexity of this use case results from the requirement of modeling a rotating region.

    Simulations involving rotating regions require a few additional steps during CAD preparation and simulation setup. We will cover the entire workflow in this tutorial.

    turbine simulation post processing
    Figure 1: Velocity vectors plotted onto the velocity field.

    This tutorial teaches how to:

    • Set up and run an incompressible water turbine simulation, making use of a rotating zone;
    • Assign boundary conditions, material, and other properties to the simulation;
    • Mesh with SimScale’s standard meshing algorithm.

    We are following the typical SimScale workflow:

    1. Prepare the CAD model for the simulation;
    2. Set up the simulation;
    3. Create the mesh;
    4. Run the simulation and analyze the results.

    1. Prepare the CAD Model and Select the Analysis Type

    To begin, click on the button below. It will copy the tutorial project containing the geometry into your Workbench.

    The following picture demonstrates what is visible after importing the tutorial project.

    Water Turbine Start view
    Figure 2: Imported CAD model of a Francis turbine in the SimScale Workbench

    The Simulation contains one geometry that consists of the Flow region of a Francis turbine and the MRF rotating zone.

    Did you know?

    Water turbines operate by removing kinetic and potential energy from the flow and converting it into mechanical torque on a shaft.

    Water pumps work in the exact opposite way. By inputting mechanical energy, in the form of torque on a shaft, pumps can pressurize the water flow.

    1.1 Geometry Preparation

    The imported geometry for this tutorial is ready for CFD simulations. Please note that it doesn’t contain any of the solid walls of the turbine. For this kind of analysis, only the flow region and rotating zone are necessary.

    In case you are interested in the workflow to prepare your turbine design for a simulation with rotating zones, consider checking the following articles:

    Creating a Cylinder in the Edit in CAD Mode

    Did you know? Rotating zones can also be created on the SimScale platform using the CAD mode. Check out this acticle in order to learn how to create a cylinder in the Edit in CAD mode.

    1.2 Create the Simulation

    To start the simulation setup process select the Francis turbine geometry to access further options.

    Water Turbine Create Simulation Selection
    Figure 3: Creating a new simulation for the Francis turbine

    Hitting the ‘Create Simulation’ button leads to the simulation type selection widget:

    types of simulation analysis available within simscale
    Figure 4: Library of analysis types available in SimScale.

    Choose ‘Incompressible’ as the analysis type and confirm the selection by clicking on ‘Create Simulation‘.

    2. Assigning the Material and Boundary Conditions

    The following picture shows an overview of the boundary conditions.

    Tutorial Water Turbine Boundary Conditions
    Figure 5: Overview of the boundary conditions for the Francis turbine geometry
    1. Volumetric Flowrate Inlet \( \dot U= 16 \frac{m^3}{s} \)
    2. Gauge Pressure Outlet \(0 Pa\)
    3. MRF rotating zone \(36.61 \frac{rad}{s}\)
    4. Rotating Wall \( 0 \frac{rad}{s} \)

    Did you know?

    The entire volume inside the MRF rotating zone is spinning at a specified rotational velocity.

    In case the rotating zone intersects a surface that shouldn’t be spinning, you can create a rotating wall boundary condition for this face, specifying a rotational velocity of 0. This will prevent the intersected parts from spinning.

    For example, in our geometry, one face that shouldn’t spin is intersected by the rotating zone:

    rotating zone intersecting face turbine
    Figure 6: MRF rotating zone (in yellow) partially intersecting a surface (in red).

    Later on, in this tutorial, the face highlighted in red will receive a rotating wall boundary condition, with a 0 \(rad/s\) rotational velocity.

    2.1 Define a Material

    This simulation will use water as fluid. Therefore click on the ‘+ button ‘ next to materials. In doing so, the SimScale fluid material library opens, as shown in the figure below:

    Water Turbine material selection
    Figure 7: Library of available fluid materials.

    Select ‘Water’ and click ‘Apply’. Keep the default values, and assign the entire Flow region to it.

    Water Turbine Assign Water Material
    Figure 8: Note that only the Flow region receives a material assignment

    The MRF rotating zone volume is not assigned to any material.

    2.2 Assign the Boundary Conditions

    In the next step, boundary conditions need to be assigned as shown in Figure 5. We need to set up and assign a velocity inlet, a pressure outlet, a rotating wall, and a rotating zone.

    2.2.1 Velocity Inlet

    Click on the ‘+ button ‘ next to boundary conditions. A drop-down menu will appear, where one can choose between different boundary conditions.

    Water Turbine Boundary Condition Selection
    Figure 9: Boundary conditions available in SimScale. From the list, choose Velocity inlet.

    After selecting ‘Velocity inlet’, we have to specify some parameters and assign faces. Please proceed as below:

    volumetric flow inlet simscale boundary condition
    Figure 10: Assigning a volumetric flow rate to the inlet.

    A volumetric flow rate of \( 16 \frac{m^3}{s}\) of water will enter the domain through the inlet face.

    2.2.2 Pressure Outlet

    The next one will be a pressure outlet. Make sure (P) Gauge pressure is set to a Fixed value of \( 0 Pa\).

    setting up a pressure outlet boundary condition
    Figure 11: The outlet face receives a fixed pressure boundary condition.

    Did you know?

    After going through the turbine runner, water exits through a section named draft tube. The purpose of this tube is to slow down the flux, converting kinetic energy into potential energy.
    The draft tube should be carefully designed, as it is directly related to kinetic energy loss at the outlet.

    2.2.3 Rotating Wall

    As previously described, one of the faces receives a rotating wall boundary condition. To achieve this create a new boundary condition and choose ‘Wall’. Set it up as shown below:

    boundary condition to prevent rotation
    Figure 12: This boundary condition prevents all parts of the selected walls from spinning.

    Remaining Walls / Surfaces

    For the remaining surface / walls no boundary conditions have to be created, as SimScale will automaticly assign a no slip boundary condition to all surfaces without a user defined boundary condition.

    2.3 Advanced Concepts: Creating a Rotating Zone

    In the left-hand side panel, navigate to Advanced concepts. Click on the ‘+ button ‘ next to Rotating zones and select ‘MRF rotating zone’. Define the MRF zone as shown:

    Water Turbine MRF Zone
    Figure 13: Rotating zone setup parameters. The entire volume within the rotating zone will have a 36.65 rad/s rotational velocity.

    Did you know?

    MRF Rotating zones are chosen in this project, as we are running a steady-state simulation.
    If we were calculating a transient problem, we would need to choose AMI Rotating Zone.
    This article provides more information about the difference between MRF and AMI Rotating Zones.

    2.4 Result Control

    Under result control, users can specify a variety of monitors, such as area averages and probe points. These are particularly useful to assess convergence and the reliability of the results. For now, let’s set up 2 result controls – we will take a look at the results later on during the tutorial.

    To assess the force and torque applied on the turbine runner blades please set a ‘Forces and moments’ control item. Assign it to a pre-defined topological entity set named ‘Runner blades’:

    Water Turbine Force Report
    Figure 14: Forces and moments control for the runner blades of the Francis turbine.

    Another important characteristic of a pump is the pressure drop. Since the outlet is set to 0 \(Pa\) the pressure at the inlet directly displays the pressure drop of the pump. Therefore create a second control item. Click on the ‘+ button’ next to Surface data. Create an ‘Area average’ control for the inlet, as shown in the picture below.

    Water Turbine Surface average report
    Figure 15: Average monitors set at the inlet and outlet.

    3. Mesh

    To create the mesh, the Standard algorithm will be used with the standard settings. In addition to the standard settings, a few mesh refinements will be created to ensure that the features of the blade and fins will be accurately captured.

    Did you know?

    It’s necessary to define cell zones whenever we want to apply a specific property, such as a rotating motion, to a subset of cells.

    Whenever Physics-based meshing is enabled for the standard mesher, the algorithm automatically creates the necessary cell zones. Since physics-based meshing is enabled in this tutorial (see Figure 19), we don’t have to worry about the cell zone definition.

    In case you are using a different mesher, the rotating zones documentation page provides alternative workflows for the cell zone definition.

    3.1 Mesh Refinements

    a. Local Element Size

    To create a mesh refinement, click on the ‘+ button ‘ next to Refinements. Choose the ‘Local element size’ from the drop-down window.

    mesh refinement standard
    Figure 16: Refinement types available for the standard algorithm

    With a ‘Local element size’ refinement, it’s possible to prescribe a maximum edge length to selected entities. Proceed as below to set up the first refinement:

    Water Turbine Mesh refinement Detailed Blades
    Figure 17: First local element size refinement. Blades with a lot of detail are selected.

    Set maximum edge length to ‘0.01’ \(m\). To save time, you can assign this first local element size refinement to a topological entity set named ‘Detailed blades’.

    b. Local Element Size 2

    Create yet another ‘Local element size’ refinement. This time we will select geometry parts that don’t require as much refinement. Input ‘0.025’ \(m\) as the Maximum edge length and assign it to the following topological entity set:

    Water Turbine Mesh refinement Runner blades and guide fins
    Figure 18: Second local element size. Parts of the guide vanes and runner are selected.

    3.2 Generating the Mesh

    Water Turbine generate mesh
    Figure 19: Next to the Generate Mesh button you’ll find an estimated time and core hour usage for the mesh generation.

    Now you can hit the ‘Generate’ button in the global mesh settings presented in Figure 19. After about 30 minutes you will receive the following mesh:

    standard mesh of a francis turbine
    Figure 20: Finished mesh using the hybrid standard meshing tool

    For more insights on mesh quality assessment, please check this page.

    Did you know?

    You can also select single faces of the geometry and hide them. This way, you can inspect inner surfaces.

    4. Start the Simulation

    Click on the ‘+ button ‘ next to Simulation Runs.

    starting a simulation in simscale
    Figure 21: Starting a simulation run.

    Now you can ‘Start’ the simulation.

    Water Turbine new run _2
    Figure 22: for every run, the estimated run duration and core hour cost are displayed.

    While the results are being calculated you can already have a look at the intermediate results in the post-processor by clicking on Solution Fields. They are being updated in real-time!

    After around 72 minutes, the turbine simulation finishes running.

    Water Turbine solution fields
    Figure 23: By clicking on Solution fields during the run, you can inspect intermediate results. After the run is finished you can also enter the post-processor through Post-process results.

    5. Post-Processing of a Turbine Simulation

    5.1 Pressure Drop

    One of the most important parameters to observe when evaluating the performance of a water turbine is how much the pressure drops after the water has flown through the turbine. You can calculate the pressure drop by subtracting the inlet pressure from the outlet pressure.

    Because you have added an Area average output for the inlet and defined a pressure outlet with 0 \(Pa\), only the pressure at the inlet is required to calculate the pressure drop.

    Water Turbine Inlet pressure Report
    Figure 24: Average pressure at the inlet of a turbine. This can be viewed below the Area average tree.

    As you can see from the figure above, the pressure still has some fluctuations therefore the average of the last values should be calculated. For example, calculate the average from time step 600 to 1000 which is approximately 1.8 \(MPa\). So, the pressure drop due to the turbine is approximately 1.8 \(MPa\).

    Find more ways to calculate the pressure drop here.

    Fluctuation of a result control Item

    Even though the simulation was run in steady-state, transient effects can still occur. Have a look at this article on how to detect transient effects in a steady state simulation.

    5.2 Forces and Moments on the Turbine Blades

    The Forces and moments results are of particular interest in a simulation with a turbine. The runner of our turbine was rotating around the y-axis. Hence, let’s inspect the resulting pressure forces and the torque generated around said axis:

    Water Turbine Force and Moment Report
    Figure 25: Pressure force (black) and torque due to pressure (blue) around the y-axis on the runner blades

    Did you know?

    The resulting torque on the blades is given by a sum of pressure, viscous and porous moments around the rotation axis.
    In this simulation, close to 293 000 \(N.m\) of torque is generated about the y-axis of the turbine.

    5.3 Particle Traces

    Streamlines can be a great tool to visualize flow patterns, especially in rotating machinery applications. Follow the steps below to show the flow streamlines inside the turbine:

    Water-Turbine-particle-trace
    Figure 26: The particle trace filter tracks the path of the fluid as it travels across the domain
    1. Remove any predefined filters and click on the ‘Particle Trace’ on the top filters ribbon.
    2. Ensure that the Pick position icon pick position button is activated.
    3. Choose the inlet as a seed for the traces.

    Now repeat the process, but this time select the outlet as a seed face.

    Water Turbine particle trace 2
    Figure 27: Tracing particles from both inlet and outlet will help to cover the entire turbine flow domain. Here, the swirl towards the outlet region can be seen as a result of rotatory turbine motion from the rotating zone.

    After the traces are created, you can adjust the render mode to ‘Translucent surfaces’ to give a better view of the flow. We can see that the flow follows a circular motion in the outlet region due to the rotatory motion of the turbine.

    5.4 Cutting Planes

    To get more details on the flow behavior inside the turbine, hide the Parts Color and create a Cutting Plane filter.

    Water Turbine cutting plane
    Figure 28: All filters in SimScale are highly customizable, allowing for a better visualization
    1. Create a ‘Cutting plane’ filter using the top ribbon.
    2. In the configuration window, change the Position of the cutting plane to ‘-0.25, 5.333, -3.029’. Furthermore, adjust the Orientation of the cutting plane to the ‘X’ direction. The Coloring of the plane is ‘Pressure’.
    3. Turn on the Vectors toggle and change the Coloring to a solid color and choose the color black. Finally, reduce the Scale factor of the vectors to ‘0.03’ and the Grid spacing to ‘0.005’.

    From the figure above, you can see how the water pressure drops when flowing inside the turbine and decreases even more after flowing to the outlet. You can also see how the blades are affecting the flow by adjusting the position and orientation accordingly. Please follow the instructions below:

    Water Turbine cutting plane 2
    Figure 29: Cutting plane showing pressure distribution inside a Francis turbine, observing the blades and guide vanes.
    1. Change the Position of the cutting plane to ‘-0.25, 2.771, -3.029’. Furthermore, adjust the Orientation of the cutting plane to the ‘Y’ direction. The Coloring of the plane is ‘Velocity Magnitude’.
    2. Adjust the Scale factor of the vectors to ‘0.05’ and the Grid spacing to ‘0.02’.
    3. Enable the Project vectors onto plane option.

    In this view, you can get insights into how the blades and guide vanes are affecting the flow, allowing for optimizations in the design.

    Analyze your results with the SimScale post-processor. Have a look at our post-processing guide to learn how to use the post-processor.

    Note

    If you have questions or suggestions, please reach out either via the forum or contact us directly.

    Last updated: October 7th, 2022

    Contents