Fill out the form to download

Required field
Required field
Not a valid email address
Required field
Required field


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.

Firstly, when a simulation is successful or 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 the ‘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. The larger the data, the longer it takes to load results.

To perform this tutorial use the project link below:


SimScale’s post-processor interface is similar to the simulation pre-processing interface. The post-processor also has general tools and filters that you can use to get the most out of your fluid 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. Go to Colouring, click on the dropdown and select one of the velocity components/magnitude.

how to change part colors in simscale
Figure 3: Follow the steps above to visualize the velocity magnitude distribution on the pipe as your starting point.

Through the legend, you can switch between quantities. The animation below shows how the Legend toggle and the legend itself can be used.

animation of changing units through the legend in simscale
Animation 1: How to toggle the legend and change the visualized quantity and its units. You can also change the range of the quantities to get a better visualization.


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.

It can be observed that velocity is zero at the walls due to the no- slip condition. Meanwhile, the velocity at the inlets is colored as per the legend.

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

Point Inspection

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

  • Select the Point inspection point inspection icon tool in the post-processor.
  • Click on the point of interest. The quantity is the value of the variable as selected in the legend along with units. As an example, place the inspection points at the outlet of the pipe.
steps to use the point inspection tool
Animation 2: 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.

By using the point inspection tool, it can be seen that the flow velocity 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 Bulk calculator.

Bulk Calculator

The Bulk calculator shows additional values on a certain face or filter such as a velocity average. To use the Bulk calculator, click on bulk calculator icon icon and then select the part or area where the calculation will be done. The bulk calculator will appear on the bottom left of the post-processor along with the quantities. For example, we will use the bulk calculator on the outlet of the pipe.

how to use the bulk calculator in simscale
Figure 4: Additional statistical calculations of pressure done with the Bulk calculator tool on the outlet of the pipe junction.

By using the Bulk calculator, 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 to an experiment or hand calculations.


To create a screenshot:

  • 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. The legend will adjust accordingly.
screenshot of simscale's screenshot tool
Figure 5: Screenshot area is bounded b the blue frame. Make sure that everything that you want to include in the picture is inside this area.
  • Finally, after the screenshot is taken, you can change the name of the screenshot and provide a short description. The image can be downloaded or deleted in the screenshot dialog box.
screenshot dialog box
Figure 6: 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 and they can be added by clicking the ‘Add filter’ button.

filters panel
Figure 7: Filters panel, where you can add/delete Filters.


These filters can be can be combined with the coloring of the parts or with each other. Each filter will have its own visibility toggle to hide or visualize it.

Cutting Planes

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

  • Click the ‘Add filter’ button at the bottom of the Filters panel.
  • Select ‘Cutting plane’. The settings of the cutting plane will appear directly below the panel.
  • Using the sliding bar, set the position of the cutting plane along the selected axis or by defining the coordinates by clicking on ‘Position’. The position of the cutting plane is represented with the following coordinates: (3.725e-9, 0.18, 0.33)
  • Orientation sets the orientation of the cutting plane by determining the normal direction.
  • Coloring defines what parameter to visualize.
  • Vectors’ toggles the visibility of vectors. You can change the colors of the vectors with a solid color or with the velocity magnitude. The size and spacing of the vectors can also be configured for accurate visualization. The size of the vectors can also be limited by defining the range of clamping. The vectors can also be filtered depending on the vector that is visualized.
cutting plane settings as one of the filters to post-process fluid flow simulation
Figure 8: 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.

We can see that recirculation occurs near the junction area in the figure above. 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:

  • Click the ‘Add filter’ button at the bottom of the Filters panel.
  • Select ‘Iso Surface’.
  • In the settings, select the flow quantity Pressure to be displayed from the list besides Iso scalar, set the Iso value as ‘-1600’ \(Pa\). The coloring is set to pressure but any other quantity can be set too including a solid color.
isosurfaces settings and example of how to use isosurfaces as one of the filters to post-process fluid flow simulation
Figure 9: Using the Iso surface filter to visualize areas where pressure is -1600 \(Pa\) and the velocity in those areas. Iso surfaces are useful when searching for unrealistic or unphysical values in the simulation

Iso surfaces can be useful in identifying critical areas such as the maximum and the minimum values. For example, in the figure above, we identified where the lowest pressure occurs, which is around the bend of the pipe.

Iso Volumes

Similar to the Iso Surface filter, the Iso Volume filter isolates volume regions in the model for a certain range. These are the steps to create iso volumes:

  • Click the ‘Add filter’ button at the bottom of the Filters panel.
  • Select ‘Iso Volume’.
  • In the settings below, select Pressure to be visualized and set the Iso value range where the minimum is ‘-1615’ \(Pa\) and the maximum is ‘0’ \(Pa\). This will display areas where the pressure is less than or equal to 0 \(Pa\).
  • ‘Vectors’ can also be shown on these volumes and the settings are similar to those for Iso surfaces.

Iso Volumes can help find regions where a quantity is over/below a certain threshold or requirement.

isovolumes settings and example of an isovolume filtering pressure below 0 pa as one of the filters to post-process fluid flow simulation
Figure 10: Iso volumes of pressure below 0 \(Pa\). Iso volume can be a great filter for isolating regions within a specified range of flow variables.

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 is often used to visualize the flow movement. Here are the steps to create Particle traces:

  • Click the ‘Add filter’ button at the bottom of the Filters panel.
  • Select ‘Particle Trace’.
  • Pick the entry position for your particle trace by clicking the icon pick position button beside Pick position. Here, we will choose the vertical inlet as the entry position of the particle traces.
  • Determine how many particle traces horizontally and vertically by sliding the toggle or entering a number beside #Seeds horizontally and #Seeds vertically. The default values will suffice.
  • Determine the distance between each streamline by configuring the Spacing. The default values can be used for now.
particle traces settings and example of particle traces going through a pipe as one of the filters to post-process fluid flow simulation
Figure 11: Particle traces of flow coming from the vertical inlet of the pipe. Streamlines can be useful when checking for recirculation or flow separation.

Streamlines can be insightful in observing the fluid flow from a certain location – it can either be defined on a specific face of the model or on a cutting plane. From the picture above you can see high \(k\) (turbulent kinetic energy) values downstream of the bend due to intermixing.

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: June 16th, 2021

What's Next

part of: SimScale Tutorials and User Guides

Data Privacy