SimScale CAE Forum

Session 2: CFD Analysis for Scavenging in the Exhaust Manifold


Homework Submission

Submitting all three homework assignments will entitle you to a certificate of participation.

Homework 2 - Deadline: 25th of June, 12pm

Submission Form


Computational Fluid Dynamics(CFD) plays a major role in IC engine design decisions such as design validation of the intake, combustion/ fuel efficiency in the cyliner, parametric studies at different exhaust mass flows and the list continues. In this exercise we focus on the CFD analysis of the scavenging process. Scavenging is the process through which the exhaust gases are forced out of the Cyliner of the IC Engine and directed out through an exhaust manifold. Now, how could CFD play a role in the design validation of an exhaust manifold? Let’s take a look.

As it is clear from the explanation above, the scavenging process is aimed at directing the exhaust gases out of the IC engine. This implies that the manifold must be designed in such a way that there is no choking/ blockages. In other words, the flow within the manifold must not be subjected to strong recirculation zones. This is where CFD comes into play. The designer can use CFD with the SimScale platform to validate a design by analyzing the flow patterns in the manifold to detect regions of strong backflow/ recirculations.

Handout Project:

This project can be used as a starting point for your simulation.

Parametric Onshape Model

You would use this parametric CAD model at a further point in this tutorial.

Submission Form

Mesh Generation

Navigate to your geometry and click on New Mesh.

Please select a Tet-dominant mesh and change the Mesh Fineness to 4-Fine. Switch the mesh fineness to 4-fine and the number of computing cores to 8. Next, click on New to add a new Mesh refinement.

Set the type to Layer Addition and set the layer addition parameters. Right click in the viewer and select all.

Next, unselect the faces on the two inlets and outlet by simply clicking on them. Add selection from viewer after the 3 faces have been unselected.

Assign a name to your refinement and Save.

Once these assignments have been made, please Start the mesh operation.

The mesh may now be visualized in the viewer.

Once the mesh is ready, we may assign the Topological entity sets A new toplogical entity set is assigned as follows:

  1. Navigate to topological entity sets in the Navigator
  2. Select the face entity from the viewer.
  3. Click on New from selection
  4. Name your entity set as you deem suitable and Create.

Please follow the above steps and this image to create the inlet1 entity.

Please follow the above steps and this image to create the inlet2 entity.

Please follow the above steps and this image to create the outlet entity.

Please follow the above steps and this image to create the Pipe entity:

  1. Hide the 3 entities you created

  2. Right Click in the viewer and select all. Click on New from selection.

  3. Assign the name Pipe and Create.

Simulation Setup

The mesh now been setup and satisfactorily analysed. The next step in your workflow is to move into the Simulation Designer. To create a new simulation, please click on New.

Please assign a name to your simulation and click Create.

Based on the fact that the maximum speeds attained by the bicylist are well below Mach 0.3 (a thumb-rule for compressibility), Incompressible can be selected as the Analysis Type.

Proceeding to Domain selection, you can select the mesh on which you want the simulation to be performed. This is particularly productive when you would like to work with different meshes.

Navigate to Materials and and click on New.

Next, add Air as the material from the Material Library.

Assign it to the volume in your mesh.

The initial conditions are assigned to the whole domain at the start of a simulation. During a simulation, the solver tries to converge the solution fields after taking these initial condition values as a starting point. Therefore, it is important to assign best guesses or analytical solutions as initial conditions when possible.

We assume a medium turbulence intensity of air (I=10%=10) for our simulation. The values of Turbulence Kinetic Energy (K) and Omega (ω) can be calculated (Formulae)*:

Turbulence Kinetic Energy (K) = 1.5
Omega (ω) = 32.06

Please feed in the values of K and omega into their respective positions in the Navigation Pane.

The overview of the physics setup is as follows:

You may now proceed to setup the physics of the simulation. To create a new boundary condition, please select Boundary Conditions in the Navigation plane and click on New.

The inlet1 boundary condition can be created as follows:

The inlet2 boundary condition can be created as follows:

Please create a New Boundary Condition. The outlet boundary condition can be created as follows:

Please create a New Boundary Condition. The Pipe boundary condition can be created as follows:

The Numerics on the platform have been optimized and do not need to be changed for this simulation. You could analyse them by selecting Numerics in the Navigation pane :

The Simulation Control provides user-control over the simulation. You can increase the Number of computing cores to 8 and Maximum runtime to 3000s.

Please note: The End time value represents the computation time and Maximum runtime represents the wall clock time (real time!)

For accurate verification of the results, additional solution fields need to be post-processed. The platform provides a Result Control panel to serve this purpose. The additional Result Control Items (solution fields) can be setup and exported as follows.

Navigate to Result Control and click on New to add a Field Calculation item.

Add the yPlus monitor as follows:

Click on New to add a Surface data monitor.

Add the AreaAvg-Inlet1 as follows:

Click on New to add a Surface data monitor.

Add the AreaAvg-Inlet2 as follows:

Click on New to add a Surface data monitor.

Add the AreaAvg-Outlet as follows:

You are now almost ready to start your simulation run. Please navigate to Simulation Runs in the Navigation pane and Check the simulation setup. If there is no error, please create a new run by clicking on New.

Please feed-in the name of your simulation.

Please click on Start to begin your simulation run.

To create the proceeding simulations, you can simply duplicate the simulation setup by right clicking on the simulation you would like to duplicate and press Duplicate. Please feed-in the name of your new simulation and click on Save.

Setting up the parametric study


The modified design of the exhaust manifold has been appended with a dent . This dent would influence the performance of the manifold. Your task is to modify the parametric dent according using a dent radius in this range: ( 0.005 m, 0.019 m). An example to modify the dent is as follows.

This is the geometry you have been provided with:

Please make a copy as follows:

Now, move to the ParametricDent tab on the bottom of your screen.

Double Click on Variable DentRadius to modify the dent.

Subsequently, update the radius within the provided range ( 0.005 m, 0.019 m).

Importing to the SimScale Platform:
Now, move back into your homework project on the SimScale platform. Navigate to Geometries and Import the model you created on Onshape:

Make sure to select 1 since you do not want to import the additional surface.

You now have your dented manifold on the platform.

The Meshing and Simulation Setup procedure remains identical to the one described for the clean exhaust manifold.


Confirmation of Convergence:

It is a common misconception that residual convergence is equivalent to solution convergence. While residual convergence is imperative for a converged solution, it is also important to monitor the convergence of various fields at different locations in the domain.

To visualize the convergence plots, please navigate to the Post-Processor in the workflow and select *Convergence plot in the Navigator.

To visualize the y-velocity convergence, select Uy under the AreaAverage-Outlet monitor.

To visualize the x-velocity convergence, select Ux under the AreaAverage-Outlet monitor.

To visualize the z-velocity convergence, select Uz under the AreaAverage-Outlet monitor.

To visualize the Turbulence Kinetic Energy (TKE) convergence, select k under the AreaAverage-Outlet monitor.

To visualize the pressure convergence, select p under the AreaAverage-Outlet monitor.

This plot might look scary but taking a closer look at the fluctuation range, it is in the order of 1e-16. The pressure field can hence be said to have converged as well.

To visualize the Turbulence Eddy Frequency, select omega under the AreaAverage-Outlet monitor.

Duplicating the result:
To add a duplicate of the result, right click on Solution fields and select Load results to viewer.

Please make the second Run 1 invisible by clicking on the eye-symbol. This first Run 1 is the simulation run on which we will be performing the post-processing. Change the Opacity to 0.5

Slices provide planar representations of Solution fields. We use the slices to analyse the solution fields at different planar locations in the manifold.

To create a new filter, select the first Run 1 and click on Add filter.

Select Slice as the filter.

The Slice can be setup as follows:

The position of the plane can be varied with the tabs Origin and Normal. Please feel free to further analyse the solution fields by tweaking the slice.


Streamlines of velocity provide a good qualitative representation of the flow reversals within the exhaust mainfold. The streamlines are represented in the Post-processor by a Stream tracer.

To add a Stream tracer, please add a New Filter and select Stream tracer

The Stream tracer may be setup as follows:

These streamline help us deduce that the manifold geometry does not have significant recirculation regions at the engine operating point under consideration. Hence, it can be said that this is a valid design at our engine operating point. But beware, this might not be the case for all engine operating points.

As a last step, we visualize the yPlus for our simulation.

The maximum yPlus is approximately 11.19. This makes it a a valid turbulent simulation setup, since we are also using wall functions to resolve the turbulence in the boundary layers.

The user is also free to analyse the results locally by downloading it to their system. An opensource post-processor, Paraview, can be downloaded here.

Thank you very much for your attention and Happy SimScaling!


PDF Version of the Workshop: CFD Analysis for Scavenging in the Exhaust Manifold


Hi @akshay_kumar,

you have to import the project into your workspace by following this link: Handout Project

Tell me if you need anything else.

All the best,


ya i have done it tq

where can i submit homework any link

Hi again @akshay_kumar,

not sure if there is any homework submission in this workshop but if so my colleague @kcontractor will soon add the submission link.

All the best,


Hi,Tmrw may 31st we need to submit our homework assignment Somebody help me to get the homework submission link…

Hi @manimaltese,

The homework link will be added by tomorrow :slight_smile:

We will also be extending the submission deadline to 25th June :slight_smile:


1 Like

Hi! Can’t find this course link to enroll in simscale academy workshop series. Could you enroll me into the course please? ill finish the homeworks by the deadline

Hi @jeettrivedi,

maybe @AnnaFless can give you more information about that. No worries you still have some time to hand in your solution :slight_smile:

Enjoy your weekend!