This tutorial showcases how to use SimScale to run an incompressible fluid flow 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 set up. 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 own workbench.
The following picture demonstrates what should be 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 are able to 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. Only the flow region and rotating zone are necessary.
In case you are interested in the process of creating the flow region and the MRF rotating zone in a CAD software, consider checking the following articles:
Select the Francis turbine geometry.
Hitting the ‘Create Simulation’ button leads to the following options:
Choose incompressible as the analysis type and ‘create the 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’. Doing so opens the properties of water, keep the defaults, and assign the entire flow region to it.
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:
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 the ‘MRF rotating zone’. Define the MRF zone as shown:
Did you know?
MRF Rotating zones are chosen in this simulation, because 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.
First, navigate to numerics. Add 2 non-orthogonal correctors to help to stabilize the simulation run.
In simulation control, enable potential foam 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 set up 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 trustability 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. 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 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 the most geometries.
Make sure it is set up as shown below. For this project, layers will be manually specified.
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:
To save time, you can assign this first local element size refinement to a previously created topological entity set.
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 maximum edge length and assign it to the following topological entity set:
c. Inflate boundary layer
The last mesh refinement, is an inflate boundary layer refinement. Follow the steps below:
Cell zones are required to apply a specific property to a subset of cells. In this case, a cell zone is required for the MRF rotating zone volume.
Click on the ‘+ button’ next to cell zones. Set it up as in the figure below:
Now you can hit the ‘generate mesh’ button in the global mesh settings presented in figure 20. After about 30 minutes you will receive the following mesh:
You can use 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 90 to 120 minutes, the 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.
By inspecting the result controls, we can evaluate how key parameters change as the iterations go on. As the simulation progresses, parameters are expected to converge to a stable result.
For a turbine geometry, some parameters of interest are:
The forces and moments results are of particular interest in simulations with turbines. 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 around the y axis.
For more information about convergence in CFD simulations, please check this article.
The picture below shows streamlines created with a particle traces filter. By using the various post-processing filters, one can gain insight into the geometry, allowing for design improvements.
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: August 13th, 2020
We appreciate and value your feedback.
