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: Post-Processing Fluid Flow Simulations

    In this tutorial, you will learn how to use SimScale’s online post-processing platform to process the results obtained from our pipe-flow onboarding tutorial. You can choose to perform the Step by Step Tutorial: Fluid Flow Simulation first and then use this as a guide for post-processing or directly import the finished tutorial and get started.

    The base project is a simple internal pipe fluid simulation, with two inlets and one outlet. Find below, in Figure 1, an overview of the physics of the simulation:

    base tutorial of pipe junction flow physics of simulation
    Figure 1: Base project. Readers who want to get started with the post-processing directly can get a quick overview of the physics of the simulation through this figure.

    To import the tutorial project, click on the button below:

    Firstly, when a simulation has results available, the run dialog box will prompt a ‘Post-process results’ button. Clicking this button or selecting ‘Solution Fields’ in the simulation tree will open the results in the online post-processor.

    accessing the post-processing environment in simscale to start post-process of fluid flow simulation
    Figure 2: Click on ‘Post-process results‘ or ‘Solution Fields’ to open the simulation result data in the online post-processor.


    The result will only load when you stay in the same tab where the Workbench is opened. The load time for the results will depend on the size of the data.


    SimScale’s post-processor interface is similar to the Workbench, keeping most of its functionalities. The post-processor also has general tools and filters that you can use to get the most out of your simulation results. To deeply understand all the features please refer to our standard document.

    Legend Toggle

    For this simulation, we are most interested in fluid velocity and pressure. Under Parts Color, you can select a parameter to plot on the boundaries of the model. Therefore, click on the dropdown and select ‘Velocity Magnitude’.

    how to change part colors in simscale
    Figure 3: Steps to visualize the velocity magnitude distribution on the pipe. The legend will be visible after selecting a scalar from the drop-down menu.

    Through the legend, you can switch between quantities. All options shown in the image below can be edited:

    legend bar functions
    Figure 4: Variety of functions added to the legend bar
    1. Minimum scale range
    2. Maximum scale range
    3. Unit displayed
    4. Scalar/vector fields
    5. By right-clicking on the legend, you have access to a variety of options such as color schemes, data sets, automatic scaling, etc.
    6. The slider on the bottom is a quick way to adjust the scale range

    Looking at figure 3, the outlet velocity is not uniform. To find out how the velocity varies at the outlet let’s use the Point inspection feature.


    Keep in mind the legend is only displayed when there are results selected. When no results or filters are selected, there is no legend visible.

    Point Inspection

    The Point inspection tool extracts a flow quantity at a certain location. To use the Point inspection tool, follow the steps below:

    steps to use the point inspection tool
    Figure 5: Steps to display a flow quantity at points of interest using the Point inspection tool. Use the point inspection tool when you want to get values at certain points of your model.
    1. Select the Point inspection point inspection icon tool in the post-processor.
    2. Click on the point of interest to inspect the local results

    By probing the velocity at the outlet, you will notice that it varies from approximately 0.4 to 2.2 \(m/s\). The variety in the outlet is caused by the shape of the pipe where it has a bend before the outlet. Now, we will try to get the average flow velocity at the outlet by using the Statistic feature.


    The Statistics feature shows additional values on a certain face or filter. Please follow the steps below to obtain the average velocity level on the outlet:

    how to use the statistics feature in simscale
    Figure 6: Additional statistical calculations of pressure done with the Bulk calculator tool on the outlet of the pipe junction.
    1. Activate the ‘Statistics’ feature
    2. Select the face of interest
    3. A window opens up with a summary of the velocity values on the selected face

    By using Statistics, not only can we get statistical values on the outlet but also the surface area of the outlet and the Volumetric Flow Rate. These values can be used to validate the simulation results of an experiment or hand calculations.


    To create a screenshot, proceed as shown below:

    screenshot of simscale's screenshot tool
    Figure 7: Screenshot area is bounded by the blue frame. Make sure that everything that you want to include in the picture is inside this area.
    • Click on the camera icon cameraicon
    • A blue frame will appear, this is the area of the screenshot. This means the area or model of interest will need to be inside this frame. Click on ‘Take screenshot’ when ready.

    After the screenshot is taken, you can change its name and provide a short description. The image can be downloaded or deleted in the screenshot dialog box.

    screenshot dialog box
    Figure 8: Screenshot dialog box. The name and description of the screenshot will be provided here.


    The saved screenshots can be accessed again under Solution fields when you want to view or download them.


    The Filters panel contains all the filtering tools we need to post-process the results.

    filters panel
    Figure 9: Filters panel, where you can add/delete Filters.


    Filters can be combined with the coloring of the parts or with each other. Each filter will have its show/hide toggle.

    Cutting Planes

    Cutting planes or slices visualize a flow quantity on a particular cross-sectional area. Follow these steps to create a cutting plane:

    cutting plane settings as one of the filters to post-process fluid flow simulation
    Figure 10: Example of applying a cutting plane with velocity vectors visualized. Cutting planes can be useful to get a general description of the flow inside the fluid domain.
    1. Click on ‘Cutting Plane’ to create a new filter
    2. The Position of the plane will remain the same, but please adjust the Orientation to the ‘X’ axis
    3. Under Coloring, you can define which parameter to visualize
    4. With ‘Vectors’ toggled on, you will see a vector field representing the flow velocity. Vectors are highly customizable, allowing you to change their Color, Scale factor, Grid spacing, amongst other options

    From figure 10, we can see that recirculation occurs near the junction area. This information will be important when redesigning the pipe to optimize the mixing.

    Iso Surfaces

    Iso Surface isolates regions in the model which match a given variable value. For example, if the user wants to know where the pressure is exactly 10 \(Pa\), Iso Surface is the choice. You can create an iso-surface by following the steps below:

    iso surface filter in simscale
    Figure 11: Using the Iso Surface filter to visualize areas where pressure is 10 \(Pa\)
    1. Create a new ‘Iso Surface’ filter by using the top filter ribbon
    2. Adjust the Iso scalar to ‘Pressure’ with an Iso value of ’10’ \(Pa\). This will highlight the regions in the domain with a pressure of 10, Coloring them with ‘Pressure’
    3. You can adjust the Render mode to give you more perspective of the highlighted regions’ location

    Iso Volumes

    The Iso Volumes filter is very similar to Iso Surfaces, but instead of highlighting a single value, the Iso Volumes filter allows you to highlight a range. These are the steps to create iso volumes:

    isovolumes settings and example of an isovolume filtering pressure below 0 pa as one of the filters to post-process fluid flow simulation
    Figure 12: Iso volumes of pressure below 0 \(Pa\). Iso volume can be a great filter for isolating regions within a specified range of flow variables.
    1. Choose an ‘Iso Volume’ filter from the top ribbon
    2. In the configuration window, select ‘Pressure’ for the Iso scalar and set the Iso value range where the minimum is ‘-1615’ \(Pa\) and the maximum is ‘0’ \(Pa\).

    Iso Volumes can help find regions where a quantity is over/below a certain threshold or requirement. From the figure above, we can see that the pressure reaches below 0 \(Pa\) around the junction, at the bend, and near the outlet. Similarly, Iso volumes can be used to isolate areas where cavitation occurs by changing the Max. iso value to the lowest allowable pressure before cavitation occurs.

    Particle Traces

    Particle Traces are similar to a dye that is injected into the flow and are often used to visualize the flow movement. Here are the steps to create Particle traces:

    particle traces settings and example of particle traces going through a pipe as one of the filters to post-process fluid flow simulation
    Figure 13: Particle traces of flow coming from the vertical inlet of the pipe. Streamlines can be useful when checking for recirculation or flow separation.
    • Create a new ‘Particle Trace’ filter
    • Make sure that the Pick Position icon pick position button is active. When it is on, you can click on a face to act as a seed face
    • Click on the main inlet face to place the seeds for the traces

    Streamlines can be insightful in observing the fluid flow from a certain location – the seed face can either be defined on one of the faces of the model or on a cutting plane.


    Once particle traces are generated, you can set them to move with an Animation filter:

    creating a new animation filter
    Figure 14: Animation filters are also handy for inspecting results of transient simulations
    1. Create a new ‘Animation’ filter
    2. Make sure to change the Animation type to ‘Particle Trace’
    3. Press the play button to start the animation

    As a result, you will see how the traces evolve through the domain:

    Animation 1: Animation of particle traces in SimScale’s post-processor

    Congratulations! You have successfully finished the post-processing tutorial for the fluid flow simulation!


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

    Last updated: February 3rd, 2023

    What's Next

    part of: SimScale Tutorials and User Guides