Tesla Valve - CFD Simulation SimFlow Tutorial

In the following tutorial you will learn how to:

We will investigate mass flow rates obtained in two configurations of the infinite tesla valve. We will create a two-dimensional model with periodic boundary conditions.

In the first part of the tutorial, we will calculate flow in the blocking direction of the valve. The flow will be forced by a prescribed pressure difference between the inlet and the outlet boundary of the periodic domain segment.

In the second part, we will simulate flow in the opposite direction, by changing the sign of the applied pressure difference. Finally, we will compare the results and the efficiency of the two configurations.

SimFlow is a general purpose CFD Software

To follow this tutorial, you will need SimFlow free version, you may download it via the following link:
Download SimFlow

Open SimFlow and create a new case named tesla_valve

Firstly we need to Download GeometryTesla_valve. The geometry will be imported in the same units as it was exported to the STEP format.

After importing geometry, it will appear in the 3D window.

The geometry is a three-dimensional volume. However, in this tutorial, we will work on a two-dimensional case. To prepare this kind of mesh, we will use the Plate (2D plane) base mesh, which should cut through the 3D volume. Therefore, we need to adjust the location of the geometry so that its center will be located on the XY plane.

Now we have to specify coordinates for the translation.

After the geometry is scaled we will not be able to see it in the 3D graphics panel. We can adjust the view by using the Fit View button.

In this fluid flow simulation, we are dealing with an internal flow problem. The imported geometry determines the bounds of the fluid domain. To inform the program where the boundaries of the inlet and outlet mesh should be created, we will use the Face Groups options. Face Groups can be created directly in the 3D graphics panel or from the Face Group geometry properties panel. In this tutorial, we will utilize the first approach.

Next, rotate the view in such a way that you will be able to see the second end of the geometry.

In the Geometry Panel we can find three Face Groups under the tesla_valve geometry. The first group, named default, contains all non-selected surfaces. These surfaces will constitute the walls of the valve. The two additional groups represent the inlet and outlet of the fluid domain. We will rename those groups to make the resulting boundary names more readable.

In order to create the mesh, we need to specify geometries features used during the meshing process.

We are going to create a mesh for a 2D fluid flow problem. The Plate base mesh is best suited for this purpose. This base mesh type will automatically take care of preparing appropriate boundaries for Z-direction.

Material Point tells the meshing algorithm on which side of the geometry the mesh is to be retained. Since we are considering flow inside the mold we need to place the material point inside the geometry.

You can specify the point location from the 3D view. Hold the CTRL key and drag the arrows to the destination.

Everything is now set up for meshing.

After the meshing process is finished the mesh should appear in the graphics window.

In this tutorial, we are simulating a valve consisting of an infinite number of segments, where the mesh represents only one segment. In this situation, fluid flow can be driven only by body forces or pressure difference between inlet and outlet (the same across all segments). We can assume, that the velocity field in each segment is the same along the whole valve. Therefore outlet from one segment will be an inlet to the next one, and the velocity profile from one boundary should be mapped onto the next one. This kind of constraint is usually called periodic boundary condition or periodic coupling . We can distinguish two main types of periodic coupling:

During the meshing process, we have not enforced conformity of meshes on the left and right boundary. Therefore, we cannot assume that faces on the left boundary are exactly matching the faces on the right boundary. Therefore, in this case, we should use the cyclic AMI boundary coupling.

Now we will create AMI coupling between the left and the right side of the valve segment.

We want to analyze incompressible turbulent flow inside the tesla valve. For this purpose, we will use the SIMPLE (simpleFoam) solver.

We are going to use the standard \(k{-}\omega \; SST\) model to handle turbulence.

As a fluid material, we will use water.

Selecting material from the Material Database will fill all inputs in the Transport Properties panel. At any time we will still be able to overwrite these values.

We will also modify the solver configuration what will increase the stability of the computational process.

This option usually improves stability and convergence but at an additional computational cost due to solving pressure equations multiple times.

We will decrease residual levels for pressure. We do not need to decrease the residual level for other variables because the pressure equation is usually the one converging last.

Velocity Dumping can prevent the solver from diverging even if nonphysical velocity would appear during the iterations.

We are simulating one segment of a periodic geometry, where values at the inlet and outlet of the domain are bounded by the cyclic constraint. In this case, we can not force fluid flow by using a standard approach, but we will use pressure jump instead. This boundary condition will force constant pressure difference between coupled boundaries.

If, after changing boundary condition type to Fixed Jump AMI you do not see the Jump input field then move to the tesla_valve_right boundary, where this input will appear. In this case, you will have to apply the pressure difference with an opposite sign. The Jump value input appears only on master boundary, which is the first boundary in the coupling.

During calculation, we can observe intermediate results on a section plane. To add sampling data on a plane we need to define plane properties and also select fields that will be sampled. Note that runtime post-processing can only be defined before starting calculations and can not be changed later on.

Additionally, to specifying section plane geometry we need to choose which results should be sampled on the surface.

Finally, we can start our computation.

To speed up the calculation process increase the number of CPUs basing on your PC capability. The free version allows you to use only 2 processors in parallel mode. To get the full version, you can use the contact form to Request 30-day Trial

Estimated computation time for 2 processors: 3 minutes

After preliminary calculation, we will continue with a more accurate algorithm. Change velocity discretization to the Linear Upwind scheme to minimize numerical diffusion affecting the results of the simulation.

Move back to Run panel and continue calculation. Note we did not remove the previous result but we use them as a starting point for computation with a higher-order scheme.

When the calculation is finished we should see a similar residual plot. Note that we can see how residual values get up when we have changed the convection scheme. This is due to the fact that different numerical scheme results in slightly different discrete equations which do not match results from previous calculations.

Slices tab appears next to the Residuals tab. Under this tab, we can preview results on the defined section plane.

Finally, we will calculate what is the mass flow rate in the flow blocking direction.

Results will be displayed in the console. The \(\phi\)φ variable is the flux through mesh faces. In the case of incompressible solvers, the flux is volumetric instead of mass flux. To obtain mass flow rate we have to multiply results by reference density.

In the next simulation, we will invert flow direction and once again compute the flow rate forced by the same pressure gradient.

We need to change the higher-order Linear Upwind scheme back to Upwind . This scheme will be again used for initial calculation since it is less accurate but more stable.

In the second run, we will investigate the results with fluid moving in the opposite direction.

We leave the rest of the configuration unchanged. Now we can start the new calculation.

Again, after preliminary calculation, we will continue with a more accurate algorithm.

Move back to Run panel and continue calculation.

When the calculation is finished we should see a similar residual plot.

As previously change tab to Slices and display velocity field. Compare results with previous velocity field. We can see that the velocity level is much higher under the same pressure gradient, which indicates that this configuration results in much smaller resistance.

Finally, we will calculate the mass flow rate for the second simulation and compare the results.

The sign of mass flow rate defines the direction of the flow. This time the value is positive because fluid flows outside the domain. We are interested only in absolute values. Check the ratio of mass flow rates between the two simulations:

\(Ratio = \frac{0.000115}{1.606e-005} \approx 7.2\)

As we can see, the 7.2 times more fluid flowing through the valve when we apply a pressure difference in the forward direction. Note that this simulation is in 2D, which means that the valve is infinitely wide and does not account the resistance from the side walls.

This concludes the tutorial, covering all the aspects we intended to showcase. To create a finely tuned presentation of the results, you may take advantage of the seamless integration with ParaView. You can easily open simulation results in ParaView with a single click from SimFlow.

In ParaView, you can perform typical and advanced postprocessing tasks such as displaying streamlines, contour plots, vector fields, line or time plots, and calculating volume or surface integrals.

To familiarize yourself with the ParaView capabilities, it’s worth checking out our video tutorial, Paraview CFD Tutorial - Advanced Postprocessing in ParaView, in which we demonstrate some of the most commonly used post-processing techniques.

Paraview CFD Tutorial - Advanced Postprocessing in ParaView