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

    Tutorial: Multiphase Flow Through a Globe Valve

    This tutorial showcases how to use SimScale to run a transient, incompressible multiphase fluid simulation of water flowing through a globe valve.

    multiphase simscale globe valve representation
    Figure 1: Transient results for a multiphase flow through a globe valve using SimScale’s Subsonic solver


    This tutorial teaches how to:

    • Set up and run a transient incompressible multiphase simulation using the subsonic solver;
    • Assign phase fractions as initial conditions;
    • Assign boundary conditions, multiple materials, and other properties to the simulation;
    • Mesh with the automatic meshing algorithm in Subsonic.

    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.

    cad model imported to workbench
    Figure 2: Imported CAD model of a globe valve in the SimScale Workbench

    The geometry consists of the actual Globe Valve. It consists of multiple parts as can be observed in the scene tree.

    1.1 Geometry Preparation

    The geometry for this tutorial is not ready for CFD simulations. It contains multiple solid parts of the valve. For a multiphase analysis, we need a single flow volume region.

    To create a flow volume click on the ‘Edit in CAD mode’ icon to enter the CAD mode.

    edit in cad mode
    Figure 3: CAD mode is an environment within SimScale that allows modifications to the existing geometry to prepare it for the simulation.

    Now perform the following steps:

    internal flow volume operation in cad mode
    Figure 4: Internal flow operation creates a volume region that fluids will occupy.
    1. Select the ‘Internal Flow Volume operation’. This will lead to a settings panel where the user needs to define a seed face and boundary faces.
    2. Assign the internal surface as a seed face.
    3. Assign the two faces at the entry and exit boundaries as boundary faces.
    4. Click ‘Apply’.

    Notice that there is a new volume entity called Flow region under the parts list at the very end (see Figure 5). This is the only region that will involve the fluid interaction and which will be required for the cfd simulation.

    To delete the remaining parts,

    1. Select ‘Flow region’
    2. Right-click to select ‘Invert selection’ from the drop-down
    3. Choose the ‘Delete’ operation under Body
    4. Click ‘Apply’.
    creating flow region in cad mode
    Figure 5: Select everything besides the flow region and delete it.

    The user will be left with only the flow region. Export this geometry and return to the Workbench.

    exporting the cad model to the Workbench from CAD mode in simscale
    Figure 6: Export the modified model to the Workbench again.

    The modified geometry (Flow region) will appear under Geometries as a copy of the original valve geometry.

    1.2 Create the Simulation

    Rename the new geometry to ‘Valve flow region’ and hit the ‘Create Simulation’ button.

    create new simulation
    Figure 7: Renaming the exported geometry and creating a new simulation for the globe valve

    This will open the simulation type selection widget:

    subsonic analysis type
    Figure 8: Library of analysis types available in SimScale. Choose the ‘Subsonic’ analysis type.

    Choose ‘Subsonic’ as the analysis type and ‘Create Simulation’.

    At this point, the simulation tree will be visible in the left-hand side panel. To run the simulation, it’s necessary to configure the simulation tree entries.

    multiphase global settings simscale
    Figure 9: Global simulation settings for the globe valve tutorial. Select ‘Transient’ Time dependency to toggle on Multiphase.

    The global simulation settings need to be adjusted for Time dependency which should be ‘Transient’ and the toggle ‘Multiphase’ as in Figure 5. This is the only way a multiphase analysis can be performed.

    We are simulating two materials, air and water. So let the number of phases be 2.

    Did you know?

    A multiphase analysis is used to simulate the time-dependent behavior of incompressible, isothermal, immiscible fluid mixtures using the VOF (Volume of Fluid) method.

    2. Pre-Processing: Setting up the Simulation

    The following picture shows an overview of the boundary conditions.

    globe  valve boundary conditions
    Figure 10: Overview of the boundary conditions acting on the valve geometry, velocity inlet, pressure outlet, and no-slip walls.

    2.1 Modeling Gravity

    For the current scenario, we will include the gravitational acceleration effects in the flow physics as well.

    modeling gravity in simscale for the globe valve tutorial
    Figure 11: Modeling gravity into the flow physics.

    Click on ‘Model’ from the simulation tree and set gy to ‘-9.81’ \(m/s^2\).

    2.2 Define a Material

    This simulation will begin with air initially present in the valve followed by water entering through the inlet. Therefore, this simulation will use air and water as two materials. Hence, click on the ‘+ button’ next to Materials. In doing so, the SimScale fluid material library opens, as shown in the figure below:

    selecting materials for multiphase analysis in simscale
    Figure 12: Library of available fluid materials in SimScale. Select ‘Water’ as the material. Repeat the procedure and select ‘Air’.

    Select ‘Water’ and click ‘Apply’. Set the associated phase quantity to ‘Phase 1’. This means water will be recognized by a phase fraction value of 1 throughout the simulation. Keep the default values, and assign the entire Flow region to it (if not already by default).

    assign water phase 1 to flow region
    Figure 13: Note that the Flow region receives a material assignment. Rename the material to ‘Water (Phase 1)’ to avoid confusion.

    Repeat the same procedure for the material air. However, the Associated phase will be ‘Phase 0’.

    assign air phase 0 to flow region
    Figure 14: This time assign air to the Flow region. Rename the material to ‘Air (Phase 0)’ to avoid confusion.

    2.2 Assign the Initial Conditions

    As mentioned above, initially only air is present. This needs to be defined as an initial condition. Click on the ‘+’ icon next to Initial conditions > Phase fractions > Subdomains and perform the following:

    initial conditions in simscale multiphase
    Figure 15: In a multiphase analysis initial conditions are used to define phase fractions, i.e. initially the quantity of air and water present.

    Ensure that the value of Phase 0 (air) is ‘1’ and Phase 1 (water) is ‘0’. Assign it to the entire flow region.

    2.3 Assign the Boundary Conditions

    In the next step, boundary conditions need to be assigned as shown in Figure 16. We have a velocity inlet and a pressure outlet. The rest are walls assigned by default.

    a. Velocity Inlet

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

    boundary condition velocity inlet globe valve multiphase
    Figure 16: Boundary conditions available in SimScale. From the list, choose ‘Velocity inlet’.

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

    velocity inlet in multiphase analysis
    Figure 17: Assign a 2e-4 \(m^3/s\) volumetric flow rate to the inlet face.

    The Globe valve receives a mixture of 25% air and 75% water. This means the fraction value of phase 0 is 0.25 and that of phase 1 is 0.75. This mixture will enter through the inlet face at a volumetric flow rate of ‘2e-4’ \(m^3/s\).

    b. Pressure Outlet

    Create a new boundary condition, this time a ‘Pressure outlet’, and select the outlet face. Make sure (P) Gauge Pressure is set to a fixed value of ‘0’ \(Pa\).

    pressure outlet in multiphase analysis
    Figure 18: The outlet face receives a fixed pressure boundary condition. For incompressible flows, the gauge pressure is considered.

    Did you know?

    A globe valve is used for regulating flow in a pipeline, consisting of a movable plug or disc element and a stationary ring seat in a generally spherical body.\(^1\)

    Unlike in the past, many modern globe valves do not have much of a spherical shape. However, the term globe valve is still used for valves that have such an internal mechanism.\(^1\)

    c. Walls

    In Subsonic analysis, all the surfaces that act as walls are automatically treated likewise by the solver itself. So there is no need to assign them separately.

    2.4 Simulation Control

    Don’t worry about the numerical settings for this simulation, as their default values are optimized. Open the simulation control settings and change the following:

    simulation control settings for the multiphase simulation in simscale
    Figure 19: Simulation control transient settings for the multiphase globe valve tutorial. End time and time step Delta t can be experimented with until desired results are achieved.
    • End time:
      • The distance between the inlet and the outlet as well as the surface area at the inlet can be calculated using the Geometry Info. Using the flow rate and the inlet area an approximate value for the inlet velocity can be calculated too.
      • For at least 3 fluid passes (fluid entering and exiting the valve) the time can be calculated as ~0.8 seconds which can be rounded off to ‘1’ second. You can run it for longer end times until a desired convergence is obtained.
    • Delta t: Keep it as ‘0.002’ seconds. The solver is robust to handle time steps over a large range of CFL number.
    • Write interval: We will write results every ’10’ time steps.
    • Maximum runtime: Transient simulations run longer. For this one set the maximum runtime to ‘8.64e4’ secs.

    Keep the remaining settings as default. To know more about how to control the simulation read in detail here.

    2.5 Result Control

    Result control allows you to observe the convergence behavior globally as well as at specific locations in the model during the calculation process. Hence, it is an important indicator of the simulation quality and the reliability of the results.

    a. Forces and Moments

    For this simulation, please set a ‘Forces and moments’ control on the “plug” of the valve. Click on the ‘+’ icon under Result control> Forces and moments to open the settings panel as shown below:

    forces and moments selection from simulation tree in simscale
    Figure 20: Forces and moments control for the plug of the valve

    Follow the steps carefully:

    • Close the settings panel.
    • Hide all the outer surfaces until the inner plug is visible.
      • To hide faces, select them and right-click to select the ‘Hide selection’ option from the drop-down. Continue until you see the plug as in Figure 21.
    activate box selection tool to select multiple faces at once
    Figure 21: Activate box selection tool helps in the quick selection of multiple faces of the CAD.
    • Open the settings panel again by clicking on ‘Forces and moments 1’ (see Figure 20).
    • Then activate the box selection tool and create a box from left to right to assign all 11 faces of the plug to this result control item.
    • Enter the center of rotation coordinates.

    c. Pressure Difference

    We can also get the pressure difference between the inlet and the outlet directly as follows:

    pressure difference calculation in simscale
    Figure 22: Static pressure difference direct calculation as a result control item
    • Click on the ‘+’ icon next to Surface data.
    • Set the inlet and outlet face pressure type to ‘Static pressure’.
    • Assign the inlet and outlet faces as shown.
    • Ensure that Apply Absolute Value is toggled on for a non-negative pressure difference.

    3. Mesh

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

    In this tutorial, a mesh fineness level of 4 will be used. If you wish to undertake a mesh refinement study, you can increase the fineness of the mesh by sliding the mesh to higher refinement levels or using the region refinements.

    automatic mesh fineness 4 in multiphase analysis
    Figure 23: Automatic mesh settings for the subsonic cartesian mesher

    Since this is a transient simulation it is recommended to start with coarse mesh settings and gradually increase if required to save on core hours.

    Did you know?

    The automesher creates a body-fitted mesh which captures most regions of interest using physics based meshing.
    If you are using the manual mesher, you can learn how to set up different parameters in this Subsonic manual meshing documentation page.

    4. Start the Simulation

    Now you can start the simulation. Click on the ‘+’ icon next to Simulation runs. This opens up a dialogue box where you can name your run and ‘Start’ the simulation.

    create a new run
    Figure 24: Simulation setup is now ready to run simulations.

    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’ or ‘Post-process results’. They are being updated in real-time!

    finished run and post-process results of globe valve
    Figure 25: During the simulation run and after it’s finished you can access the post-processor by clicking on ‘Solution Fields’ or ‘Post-process results’.

    Depending on the instance chosen by the machine, it might take 5-10 minutes for the simulation to finish.

    5. Post-Processing

    5.1 Visualizing the Mesh

    Once inside the post-processor, under the Parts Color filter change Coloring to any solid color of choice and then change the render mode to Surfaces with mesh to show opaque surfaces of the CAD model with the mesh grid.

    parts color surface with mesh simscale online post-processor
    Figure 26: Mesh visualization inside SimScale’s online post-processor

    You can use the cutting plane filter to see the inside of the mesh generated:

    cutting plane filter mesh solid color
    Figure 27: Inspecting the mesh in detail using a cutting plane
    1. Hit the ‘Cutting Plane’ filter from the top ribbon.
    2. Adjust the position accordingly.
    3. Adjust the orientation to ‘X’ axis.
    4. Change the Coloring to some contrasting solid color.
    5. Toggle on Show mesh so that the mesh can be visible.

    After a few seconds, you will see a clip showing the inside of your mesh. This mesh looks sufficient for this tutorial.

    5.2 Forces and Moments on the Plug

    The Forces and moments results are of particular interest in a simulation with a valve. The plug will be subjected to pressure forces from the incoming water. Hence, let’s inspect the resulting pressure forces and moments on the plug:

    forces and moments plot transient analysis multiphase globe valve
    Figure 28: Forces and moments acting on the plug of the valve are shown here against time.

    Figure 28 shows multiple runs performed with end times of 0.5, 1, and 2 seconds. For this tutorial purposes (end time of 1 second) the curves seem to be still fluctuating and more time steps might be required until a predictable pattern is observed.

    5.3 Pressure Drop

    One of the most important parameters to observe when evaluating the performance of a globe valve is how much the pressure drops after the water has flown through the valve.

    pressure difference direct plot transient analysis multiphase globe valve
    Figure 29: Pressure difference between the inlet and the outlet as set up under the result control can be visualized here.

    The transient nature of the pressure difference curve seems to be converging towards the end. Like the force plot, more time steps might be required to confirm a predictable pattern.

    5.4 Particle Traces

    Streamlines can be a great tool to visualize flow patterns. Follow the steps below to show the flow streamlines inside the valve:

    particle traces on multiphase globe valve
    Figure 30: The particle trace filter tracks the path of the fluid as it travels across the domain
    1. Remove any predefined filters and click on ‘Particle Trace’ on the top filters ribbon.
    2. Ensure that the Pick position icon pick position button is activated.
    3. Ensure that the front view for the geometry is aligned with the plane of your screen.
    4. Choose the inlet as the seed face for the traces to be generated.

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

    particle traces on multiphase globe valve translucent surfaces
    Figure 31: Tracing particles from both inlet and outlet will help to cover the entire valve flow domain. Here, the swirl toward the outlet region can be observed.

    After the traces are created, you can adjust the render mode to ‘Translucent surfaces’ to give you a better view of the flow. Similarly, you can adjust the color of the parts for a better representation.

    We can see that the flow follows a circular motion in the outlet region due to the rotatory motion of the turbine.

    5.5 Pressure, Phase Fraction, and Velocity Vectors


    To get more details on the flow behavior inside the valve, use the Cutting plane filter.

    cutting plane total pressure multiphase globe valve simscale
    Figure 32: All filters in SimScale are highly customizable, allowing for better visualization. Cutting plane showing total pressure distribution (inlet on right).
    1. Create a ‘Cutting plane’ filter using the top ribbon.
    2. Adjust the Orientation of the cutting plane to the ‘Z’ direction.
    3. Set the Coloring of the plane to ‘Total Pressure’.

    From Figure 32, you can see how the total pressure drops after the fluid air-water mixture crosses the valve plug section in the center and keeps decreasing towards the outlet.

    Phase Fraction

    Different parameters can be viewed by changing the coloring. In Figure 33 air is visualized on the same cutting plane:

    air phase fraction cutting plane globe valve multiphase
    Figure 33: Cutting plane showing air (phase fraction 0) distribution across the globe at the end of the simulation. Most of the pure air is present on top.

    In Figure 34 water is visualized on the same cutting plane:

    water phase fraction cutting plane globe valve multiphase
    Figure 34: Cutting plane showing water (phase fraction 1) distribution across the globe at the end of the simulation.

    Figures 33 and 34 complement each other with their information. Most of the valve is filled with the air-water mixture with a water fraction between 0.6-0.8 and an air fraction between 0.2-0.4. The top part of the valve surrounding the plug has more air content.

    Velocity Vectors

    Vectors can also be interpreted on the cutting plane to understand the flow patterns.

    vectors cutting plane multiphase globe valve
    Figure 35: More information can be obtained from cutting planes using vectors. They can be colored based on other parameters as well.
    • Adjust the Orientation of the cutting plane to the ‘X’ direction.
    • Change the Coloring of the plane to ‘Velocity Magnitude’.
    • Toggle on Vectors and base its coloring with any contrasting solid color.
    • Adjust the Scale factor of the vectors to ‘0.07’ and the Grid spacing to ‘0.018’.
    • Enable the Project vectors onto plane option.

    Longer vector lengths signify higher velocity magnitudes. The flow is not strong towards the bottom and top. Now change the orientation to the other two planes for more insights.

    5.6 Animation

    Any effect of the applied filters can be animated. Select ‘Animation’ from the top filter ribbon and click the play button under the Animation settings panel. Operate the animation commands as per your interests. Learn more.

    animation control panel in simscale for multiphase globe valve
    Figure 36: Animation controls
    Animation 1: Air-water mixture entering the valve from the inlet (right) from first to last time step.

    In this view, you can get insights into how the filling up of the globe valve takes place and what internal part designs 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.


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

    Last updated: May 30th, 2023