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.
This tutorial teaches how to:
We are following the typical SimScale workflow:
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.
The geometry consists of the Flow region of a Francis turbine. Furthermore, there’s also a solid cylinder part named 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.
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:
Select the Francis turbine geometry to access further options.
Hitting the ‘Create Simulation’ button leads to the simulation type selection widget:
Choose ‘Incompressible’ as the analysis type and ‘Create a Simulation‘.
The following picture shows an overview of the boundary conditions.
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:
This simulation will use water as a material. Therefore click on the ‘+ button’ next to materials. In doing so, the SimScale fluid material library opens, as shown in the figure below:
Select ‘Water’ and click ‘Apply’. Keep the default values, and assign the entire Flow region to it.
The MRF rotating zone volume is not assigned to any material.
In the next step, boundary conditions need to be assigned as shown in Figure 5. We have a velocity inlet, a pressure outlet, a rotating wall, no-slip walls, and a rotating zone.
Click on the ‘+ button’ next to boundary conditions. A drop-down menu will appear, where one can choose between different boundary conditions.
After selecting ‘Velocity inlet’, the user has to specify some parameters and assign faces. Please proceed as below:
A volumetric flow rate of ’16’ \(m^3/s\) of water will enter the domain through the inlet face.
The next one will be a pressure outlet. Make sure (P) gauge pressure is set to fixed value = 0.
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.
As previously described, one of the faces will receive a rotating wall boundary condition. Therefore, create a new boundary condition and choose ‘Wall’. Set it up as below:
The remaining solid walls will receive a no-slip condition. We can make use of SimScale’s quick selection tools to save time. A topological entity set will be created, as this set of faces will be used again during the setup. Topological entity sets allow the user to re-select a group of faces in a single click.
Please follow these steps:
Afterward, create a wall boundary condition and assign it to the newly created topological entity set.
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:
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.
Firstly, navigate to Numerics. Add ‘2’ Non-orthogonal correctors to help to stabilize the simulation run, and also adjust the Relaxation type to ‘Automatic’.
Under Simulation control, please enable Potential flow initialization. This enhances stability for velocity-driven flows, especially during early iterations. Change both End time and Write interval to ‘600’ iterations. Furthermore, the Maximum runtime should be ‘30000’ seconds.
For more information about the setup of the simulation control parameters in CFD simulations, check this article.
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 3 result controls – we will take a look at the results later on during the tutorial.
Please set a ‘Forces and moments’ control item. Assign it to a pre-defined topological entity set named ‘Runner blades’:
For the second control, click on the ‘+ button’ next to Surface data. Create an ‘Area average’ control for the inlet and another one for the outlet, as shown in the picture below.
Repeat the process, but this time for the outlet.
To create the mesh, we recommend using the Standard algorithm, which is a good choice in general as it is quite automated and delivers good results for most geometries.
Make sure it is set up as shown below. For this project, layers will be manually specified.
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 21), 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.
a. Local Element Size
To create a mesh refinement, click on the ‘+ button’ next to Refinements. Choose one of the options from the drop-down window.
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:
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 refinement 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:
Now you can hit the ‘Generate’ button in the global mesh settings presented in Figure 21. After about 30 minutes you will receive the following mesh:
You can use a mesh clip to check the quality of your mesh, as shown in the figure below:
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.
Click on the ‘+ button’ next to Simulation Runs.
Now you can ‘Start’ the simulation. 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 120 minutes, the turbine simulation finishes running. The figure below shows a run time of 274 minutes because we ran a total of 2000 iterations, to assure the results were indeed stable. However, fewer steps are sufficient and you can save some core hours.
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 outlet, you will only need to get the pressure (p) value from here and subtract the two. However, since you defined a pressure outlet with 0 \(Pa\), only the pressure at the inlet is required.
As you can see from the figure above, the pressure still has some fluctuations. Calculate the average for these values. For example, calculate the average from time step 1600 to 2000 which is approximately 1.9 \(MPa\). So, the pressure drop due to the turbine is approximately 1.9 \(MPa\).
Find more ways to calculate the pressure drop here
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:
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 187 500 \(N.m\) of torque is generated about the y-axis of the turbine.
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:
is activatedNow repeat the process, but this time select the outlet as a seed face.
After the traces are created, you can adjust the render mode to ‘Translucent surfaces’ to give you 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.
To get more details on the flow behavior inside the turbine, use the Cutting plane filter.
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:
In this view, you can get insights on 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: January 28th, 2022
We appreciate and value your feedback.
