Fill out the form to download

Required field
Required field
Not a valid email address
Required field

Documentation

Tutorial: Fluid Flow Through a Non-Return Valve

This article provides a step-by-step tutorial for a fluid dynamic simulation of a non-return valve.

non return valve illustration of a fluid flowing
Figure 1: Particle traces through a non-return valve

Overview

Valves under particular flow conditions can be simulated to obtain key performance quantities such as pressure drop through the system. Additionally, velocity and pressure results can be inspected in detail to identify regions of extreme pressure and flow inefficiencies. This tutorial acts as a guide for valve analysis best practices and can be used as a template for your future projects.

We are following the typical SimScale workflow:

  1. Preparing the CAD model for the simulation.
  2. Setting up the simulation.
  3. Creating the mesh.
  4. Run the simulation and analyze the results.

1. Prepare the CAD Model and Select the Analysis Type

First of all, click the button below. It will copy the tutorial project containing the geometry into your workbench.

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

workbench with non return valve simulation
Figure 2: Imported CAD model of a non-return valve in the SimScale workbench.

You will notice that we are only modeling one-half of the valve geometry. Taking advantage of the symmetrical nature of the valve is a great way to save on both mesh size and simulation run time.

1.1 CAD Mode

The initial geometry contains a volume that represents the body of the valve. Before we can begin a simulation, first we have to create the fluid volume. To do this, we are going to enter SimScale’s CAD mode environment:

entering simscale cad mode valve
Figure 3: To enter the CAD mode environment, select the geometry and click on the highlighted icon.

Within the CAD mode environment, we have two main goals:

  • Create an Internal Flow Volume
  • Delete the solid body of the valve

The first objective requires an Internal Flow Region operation, with the steps shown below:

creating an internal flow volume for a valve in cad mode
Figure 4: Steps for the open flow volume creation. For this tutorial, we don’t need to assign anything to Excluded Parts.
  1. Select an ‘Internal Flow Volume’ operation.
  2. Select a Seed face, which can be any internal face that will be in contact with the flow region. In Figure 4, the selected seed face is highlighted in light blue.
  3. Define boundary faces of the geometry (where the holes are). In our case, we have the two boundaries highlighted in white in Figure 4. In case you are in doubt about the boundary faces of your geometry, consider visiting this page.
  4. Hit ‘Apply’ to run the operation.

After the operation runs, you will notice that we have one additional volume: the Flow region. For single-region analysis types, such as incompressible, this is the only volume that we need to run the simulation. Now, our goal is to delete the body of the valve with a Delete Body operation:

delete body operation cad mode simscale valve
Figure 5: After deleting the valve body, you can export the new CAD model directly to your Workbench by clicking on Finish, in the top-right.
  1. Create a ‘Delete Body’ operation.
  2. Select the ‘Valve body’ volume to delete.
  3. Hit ‘Apply’.
  4. Press ‘Finish’ to export the final model to your Workbench.

1.2 Create a Simulation

In the Geometries tab, you will see a second geometry named Copy of Non-return valve. This is the one that we are going to use to run the simulation. We can change the name of the new model to something more representative before creating a new simulation. Therefore, please proceed as below:

new simulation option
Figure 6: If you wish, you can change the name of the geometry and click on the check icon to save, before starting a new simulation.
  1. Change the name of the new CAD model to Non-return valve – Flow region
  2. Click on the ‘Check’ icon to save
  3. Now we are ready to click on ‘Create a Simulation’

At this point, the analysis type selection widget opens up:

analysis type widget containing the available physics
Figure 7: Analysis type selection widget. This simulation will be an incompressible analysis

In this simulation, we calculate the flow of water through a valve. As long as the speed of the fluid is subsonic (Mach Number below 0.3), we select the incompressible analysis and create the simulation.

2. Assign Materials and Boundary Conditions

2.1 Define a Material

simscale material options
Figure 8: The Materials library contains a series of pre-defined fluid materials.

To apply the material to the geometry, press the ‘+ button‘ next to Materials to open a list with options. For this simulation, we will select ‘Water‘ and press ‘Apply‘ to confirm the selection.

Since we have a single volume, the material is automatically assigned to our flow region. Therefore, we can proceed to the boundary condition set up.

2.2 Assign Boundary Conditions

In the next step, boundary conditions need to be assigned. Here, the goal is to define the physics of the simulation, including inlet, outlet, symmetry plane, and physical walls.

To have an overview, the following picture shows the boundary conditions applied for this simulation:

non return valve boundary conditions
Figure 9: Overview of the boundary conditions for the non-return valve

a. Flow Conditions

Starting with the flow conditions, one needs to assign a Pressure inlet condition to the inlet as shown below:

pressure inlet setup
Figure 10: To create a new boundary condition, simply click on the + button.

After hitting the ‘+ button’ next to boundary conditions there will pop up a drop-down menu where one can choose between different boundary conditions.

Assign a Pressure inlet condition with a total gauge pressure of 3e+5 \(Pa\):

pressure inlet boundary condition
Figure 11: After defining the correct pressure, you can click on the appropriate face to assign it to the boundary condition.

Lastly, we will assign a Pressure outlet condition with a fixed value of 0 gauge pressure to the outlet. This sets the outlet to atmospheric pressure allowing flow to exit freely.

To create a pressure outlet boundary condition, you can follow the same steps from figure 10.

pressure outlet boundary condition
Figure 12: The combination of total pressure inlet and fixed pressure outlet is known for being very stable.

From the flow standpoint, these are the only two boundary conditions necessary. We can now define the symmetry condition for the geometry.

b. Geometry Conditions

Assign Symmetry conditions to all the surfaces that lie directly on the plane of symmetry.

symmetry boundary condition
Figure 13: Assign the symmetry condition.

2.3 Simulation Control and Result Control

Please navigate to Simulation Control in the simulation tree. The Simulation control tab allows you to change several settings, including the number of iterations and maximum runtime for the simulation.

For this tutorial, we are going to change both End Time and Write Interval to ‘2500’. With these settings, we will run a total of 2500 iterations and write only the final result set.

simulation control settings valve
Figure 14: By allowing more iterations for the simulation, it can converge more tightly.

You can also use Result controls to observe the convergence behavior of certain items of interest. In this simulation, let’s keep track of the inlet values by setting an Area average result control. Please follow the steps below:

area average result control valve
Figure 15: Area average result controls are very useful to assess convergence of a simulation.

3. Mesh

To get the mesh, we recommend using the Standard algorithm, which is a good choice in general because it is quite automated and delivers good results for most geometries.

For this initial analysis, we are going to create a standard mesh with default settings. Therefore, simply click on ‘Generate’ within the mesh setup window.

mesh menu in simscale
Figure 16: Standard mesh menu. By clicking on Generate, you will initialize the meshing process.

Did you know?

Often, large changes in the mesh’s cell sizes are only spotted in a few regions. Increasing the global mesh refinements rises the cells drastically.
When using the standard mesher, SimScale offers the option of physics-based meshing. This algorithm detects regions that require a finer resolution based on the boundary conditions set.
You can also do this manually, by using one of the local refinement options, such as local element size and region refinements.

After a few minutes, the mesh finishes running and will have the following aspect:

mesh appearance valve simulation standard tool
Figure 17: Mesh result, highlighting the non-return valve region

4. Start the Simulation

simulation tree in simscale
Figure 18: Simulation setup tree before starting the simulation.

Now you can ‘Start’ the simulation, and after 1 to 2 hours, you can have a look at the results.

5. Post-Processing

Once your simulation is complete you can use the online post-processor to visualize the results. To become more familiar with the post-processor, please refer to the following documentation.

Before jumping into the post-processor, it’s a good practice to evaluate the convergence of the simulation. In this sense, the result controls are very valuable. For example, let’s check if the velocity is stable at the inlet of the system, by inspecting the y-component:

result control convergence valve simulation
Figure 19: The stabilization trend indicates convergence. The velocity stabilizes at around 10 m/s at the inlet.

When analyzing valves, it is interesting to calculate the pressure drop and observe the velocity behavior through the system and whether any backflow occurs.

a. Pressure Drop

The pressure drop across the valve is computed by using the Cutting plane filter and the bulk calculator. Here are the steps:

  • Make sure that there are no predefined filters and that you are at the last time step
  • Select the ‘Cutting Plane’ filter in the Filters panel
filters panel with the available filters in simscale's post-processor
Figure 20: Selecting the ‘Cutting Plane’ filter from the filters panel
  • Change the Orientation of the cutting plane in the y-direction by clicking on ‘Y’.
  • Place the cutting plane upstream of the valve with the Position: -0.213, -0.05, -0.032.
  • Whenever using the bulk calculator, it’s recommended to switch the data set to cell data. To do that, you can right-click on the legend and ‘Switch to cell data’. The image below shows the steps:
cutting plane upstream of the valve
Figure 21: Cell data represents the raw data that comes directly from the solver, without any interpolations.
  • Now we are ready to toggle on the bulk calculator, by following the steps in Figure 22. A box containing information will appear on the bottom-left corner of the viewer.
bulk calculator valve simulation pressure drop
Figure 22: The bulk calculator provides minimum, maximum, and average values about the cutting plane.

In this initial analysis, the average pressure upstream of the pipe is 2.534e+5 \(Pa\).

Following the steps above, we can obtain the pressure downstream of the valve. This time, the Orientation of the cutting plane will be in the ‘X’ normal direction with the Position: -0.3, -0.022, -0.032. Both cutting planes can be seen in the figure below:

cutting plane downstream of the pipe
Figure 23: With a similar approach, we can obtain the average pressure values just downstream of the non-return valve.

From the figure above, the average pressure downstream of the valve is 649.1 \(Pa\). Therefore, the pressure drop across the valve is 2.528e+5 \(Pa\).

Find more ways to calculate the pressure drop here.

b. Backflows

Backflow is another phenomenon that is important when evaluating a valve. This is done by slicing the valve on the appropriate axis.

  • Choose the ‘Cutting Plane’ filter in the Filters panel
  • The next step is to change the orientation of the cutting plane to the ‘X’ axis
  • Next, change the Position of the cutting plane to the following coordinates: 0.02, -0.022, -0.032
  • After that, enable the slider beside Vectors. This allows you to visualize the velocity vectors. Change the Scale factor to ‘0.02’ and the Grid spacing to ‘7.5e-3’
  • At this point, you can also change the Coloring of the vectors. In Figure 23, we are using black for the vectors
  • Finally, enable the Project vectors onto plane option. The resulting cutting plane will be similar to the figure below:
cutting plane recirculation patterns
Figure 24: Cutting plane with velocity vectors visualized to show backflows and swirls

We can see from the figure above that there is backflow occurring near the entrance of the valve and there are swirls inside of the pipe. This is critical to the valve performance as it hinders the flow patterns at critical locations affecting the desired pressure drop.

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

Congratulations! You finished the tutorial!

Need a hand?

We understand that imitating tutorials might not be an easy task and that’s why in extension to the documentation we have created video tutorials to ease your efforts and help finish them successfully. The video for the above tutorial can be found here.

Note

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

Last updated: July 19th, 2021

Contents
Data Privacy