Session-1 Homework: Aircraft Cabin Ventilation


#1

Recording

Homework submission

Submitting all three homework assignments will qualify you for a free Professional Training (value of 500€) as well as a certificate of participation.

Homework 1 - Deadline 21.07 12:00pm

Form

Exercise

This exercise involves simulating the ventilation inside an aircraft cabin. For simplicity and reduced computation there is only one row of seats in the geometry. The task is quite interesting, to setup 6 different configurations by having various configurations of inlet and outlet, and then to compare the results. The possible inlets and outlets are as shown in the following figure.

The different combinations for performing the simulations are

Step-by-Step

Import the project by clicking the link below. ( Crtl + Click to open in a new tab )

Click to Import the Homework Project

Once the project is imported, the workbench is automatically opened. Then follow the steps below for setting up an incompressible flow simulation.

Meshing

  • In the ‘Mesh Creator’ tab, click on the geometry ‘Aircraft cabin’
  • Then, click on ‘New Mesh’ button in the options panel.

  • Select Hex-dominant automatic for internal flow (only CFD) mesh and select the following parameters - Moderate fineness and 8 cores. This operation will automatically create a mesh for fluid flow simulation. The cell size and refinement will be adapted automatically.

  • Since this is expected to be a turbulent flow, layers are required for all the faces except the symmetry walls. Prism layer cells are characterized by very flat elements that are able to resolve the boundary layer appropriately.
  • First click the ‘Selection’ drop down list from the tool bar and click on ‘Select all
  • Then click the 2 symmetry faces to de-select them.

  • Click the Add selection from viewer button [1] and select Save [2].
  • Now click the Start button [3] to begin the mesh operation. The meshing job will start in a few moments and all computation is done via cloud computing.

  • The mesh operation takes about 15 minutes to complete and gives a ‘Finished’ status in the lower left once it is over.

Simulation Setup

  • For setting up the simulation switch to the Simulation Designer tab and select New simulation.

  • Select the analysis type: Incompressible under Fluid dynamics.
  • Select k-omega SST as the turbulence model and Steady-state type and click Save button.
  • The flow in aircraft cabin is assumed to be Incompressible due to low velocities of the circulated air. Choosing Steady-State option means that we will simulate the Time-Independent solution.

  • After saving, the simulation tree now looks as shown below. Here the Tree Entries in Red must be completed.

Domain selection

  • Click ‘Domain’ from the tree and select the mesh created from the previous task. Click the Save button. The mesh will then automatically load in the viewer.

Create Topological Entity Sets

  • In this homework we are going to perform 6 different simulations, as discussed earlier. The image below shows various settings for inlet and outlets. It is convenient to name these under ‘Topological Entity Sets’ to be used later during the setup.

  • We will create 7 sets in total, as shown below:

  • Click on the tree entry ‘Topological Entity Sets’.
Inlet Set 1:
  • To create the first set, click the shown surfaces and click on the ‘New from selection’ button to create a set named ‘Inlet Set 1’.

Inlet Set 2:
  • Similarly, select the shown surfaces and create a new set named ‘Inlet Set 2’.

Inlet Set 3:
  • and then the shown surfaces for the third inlet set.

Outlet Set 1:
  • For the outlets, select the shown surfaces and click ‘New from selection’ button to create a set named ‘Outlet Set 1’.

Outlet Set 2:
  • Similarly for the second outlet set.

Symmetry:
  • Select the shown faces and create a set named ‘Symmetry’.

Walls:
  • Now select each created set and hide it from the viewer, as shown in the image below. This would enable us to select all the remaining faces as ‘Walls’.

  • From the toolbar click on ‘selection’ and click ‘Select all’. Then create the last set and name it as Walls.

Select Fluid Material

  • Select ‘Material’ from the sub-tree and click New.

  • Select Import from material library in the top of the pane.

  • Click Air and select the Save button.

  • Select region0 from Topological Mapping and click the Save button.

Initial Conditions

  • Under ‘Initial condition’ from the tree, select k and Omega and enter the values as shown in the following figures. Click the Save button everytime.

Boundary Conditions

The boundary conditions define the flow variables at the boundary surfaces.

  • Click on ‘Boundary condition’ and select New.

Inlet :
  • Enter the inlet boundary condition with a volume flow rate of 0.02975 cu.m/s. Select the Inlet set 1 entity and click Save option.

  • The inlet volume flow rate for Configuration 3 and 6 are maintained to be 0.07105 cu.m/s. The values are calculated such that a velocity of 0.35m/s is obtained in all cases.
Outlet :

As the velocity is not known at the outlet faces, we would define the pressure here.

  • Define a pressure outlet boundary condition to Outlet set 1 and click Save.

Symmetry :
  • Next we will define the symmetry condition.

Walls :
  • The remaining boundary definition is for the walls. One important thing to be noted is that this condition has to be assigned to all entities which are not defined the previous 3 conditions.

  • Hence for Configuration-1 setup ‘Inlet set 2’, ‘Inlet set 3’ and ‘Outlet set 2’ are also considered as walls.

Numerics

  • Select ‘Numerics’ from the sub-tree and enter the following values. This enhances the solver to get the appropriate results.

  • Set the relaxation factors to:

P : 0.3
U : 0.7
k : 0.5
Omega : 0.5

  • Set ‘GAMG’ solver for pressure with 2 pre and 1 post sweep.

  • Set ‘Smooth Solver’ for the rest with the shown settings.

  • Set the ‘Numerical scheme’ for Div(Phi,U) to ‘bounded Gauss Upwind

Simulation Control

  • Click on ‘Simulation control’ and setup the simulation run for 2000s time with a time step of 1.

Create New Run
  • Click on Simulation runs and create a new run.

.

Create Further Configurations

  • Similarly create 5 other configurations (2-6) with the following conditions.

  • You can ‘duplicate’ the previous simulation setup by right clicking and selecting duplicate. Then change the boundary conditions. Make sure not just to set the inlet and outlet conditions, but also the wall boundary condition assignments need to be changed (all the faces except inlet, outlet and symmetry) each time.

  • Only the Symmetry boundary condition assignment remains unchanged.

aerospace, aircraft cabin ventilation, inlet outlet configuration, boundary conditions

  • The simulation takes between 90 to 100 mins to finish.

Post-processing

  • Once the simulation is over switch to obtain the results by clicking on Post-process results under Results.

Slice Filter (2D):

  • Select the solution field (‘Configuration 1’ in our case) and click Add filter option and select Slice.

  • Apply the following slice properties and click the ‘Tick’ icon to apply.
    Slice type - Plane
    Origin - default values (1.213, 1.026, 0.650)
    Normal - (1, 0, 0)

  • Then Rotate in the viewer to visualize the slice.

  • Select the velocity data U [point data] - go to the last step as shown below.

  • Click on the ‘Color bar’ below the selection panel to view the ‘legend’ bar and re-scale it to data range.

Clip Filter:

  • A clip of the domain (3D) can be obtained by clicking on Add filter and selecting Clip option. Enter the following values and click the ‘Tick’ icon to apply.
    Clip type - Plane
    Origin - default values (1.213, 1.026, 0.650)
    Normal - (0, 1, 0)

Streamlines:

  • Click on the solution field (Configuration 1), Add filter and then select Stream tracer in order to get the flow streamlines. Change the display field to U [point data] and enter the following values to create a line source stream tracer (Please leave the other properties with default values).
    Vectors - U
    Maximum Streamline Length - 10
    Seed Type - High Resolution Line Source
    Point1 - (1.225, 1.75, -0.2)
    Point2 - (1.225, 1.75, 1.5)
    Resolution - 100

  • and click the ‘Tick’ icon to apply.

Velocity Vectors:

  • Glyphs can be added to get an overview of how the velocity vectors look like. This can be done by clicking on Add filter and selecting Glyph. Enter the following property values.
    Glyph type - Arrow
    Scalars - None
    Vectors - U
    Scale factor - 0.15

  • and click the ‘Tick’ icon to apply.

  • Similarly perform the post-processing of the configurations and compare!

Community Digest July 2016
#2

#3

#5

Hi @sjesu_rajendra @Milad_Mafi, in the Clip Filter section, for the plane selection should be negative for Y axis, [Normal - (0, -1, 0)], that worked for me.

Best, ML.


#6

Is there anybody else that get’s the following error while trying to run the simulation:
“The job execution was aborted. A possible cause is that not enough memory was available. In this case, selecting a larger instance or using a coarser mesh should resolve the issue.”
I double checked everything and also tried to run it with 32 cores instead of 16 but nothing resolved the problem.


#7

@GeertL - what I can definitely say is this error message is missleading - it’s NOT the machine size that’s causing the sim to fail. This missleading error message will be fixed soon but currently is hinting into the wrong direction.

The sim throws a floating point exception which hints towards some setup error, but I could not yet find it. Will report back in a bit.


#8

Hello @mlarreta,

The ‘Clip Filter’ (shown in the tutorial) can be done in either of these 2 ways.

  1. As you had mentioned, the plane selection can be negative for Y axis, i.e Normal (0, -1, 0).

  2. The one in this tutorial - Use the Normal (0, 1, 0) and then check the Inside Out to ‘True’.

It is good to know that you tried the different approach! :slight_smile:

Sam


#9

I selected the k omega analysis type whereas it had to be the k omega SST, so you’re right about the error message being kind of misleading.


#10

Glad to see that it solved the issue @GeertL


#11

Hi @sjesu_rajendra,

I have questions concerning our numeric properties. Firstly, can you please explain why we use symGaussSeidel and not just GaussSeidel?

Secondly, I would like to know why just div(phi,U) is set as bounded Gauss upwind.

Thanks in advance! :slight_smile:

Jousef


#12

Hi, while meshing I get these two error messages in the log:

Illegal
triangles were found after surface tesselation. There could be a
problem with the CAD geometry. Trying to proceed anyway

The
tesselated surface is not closed. There could be a problem with the CAD
geometry (such as self-intersections). Please inspect your geometry.
Trying to proceed anyway.

I tried to create the mesh with comouting on more cores but without any success. Now I cannot select this mesh as a domain. Thank you for any help


#13

Hello everyone,

I have the same problem as “hfoester” when trying to create the mesh.
The same two messages appear informing that problems in the surface tesselation have been found and that there must be a problem in the CAD geometry, as a result of not being a fully-closed surface.

Consequently it does not allow me to select a domain mesh in the “Domain selection” step.

Any idea how to solve this problem?

Thank you very much in advanced.

Ovi.


#14

@Ovi and @hfoester, You wont be able to select a domain until a mesh is successfully finished. I also got the warning (not error) regarding the geometry but my simulation went through anyways. In order for the issue to be found the best way to go about it is to post the project so we can have a look at it and see what is wrong. I tried to have a peak at @hfoester simulation and I confirmed that there was some sort of error in the mesh beyond the geometry warning I had so you wont be able to select a mesh for your domain. I am unsure what causes the error but I strongly advice against starting a simulation setup before the mesh is done, every single time I have done this the file gets corrupted and I end up having to start the whole thing from zero.


#15

Thanks for your answer and help @oscarcorripio. I have tried to do it again from scratch and this time it has worked without problems.

To be honest, I have no idea what it could be wrong before.

Greetings.


#16

Thank you for your support, guys!
Now the meshing is finished without any error. The simplest method of solving software or computer fails (shut down and restart) has worked fine :wink:


#17

I am sorry for bothering again, but I wanted to know if anybody else has had the same problem as I do while running the simulations.

The simulation run works well until minute 51, where it suddendly stops and a message appears indicating: “Maximum execution time exceeded”. Therefore the final status of my simulations is: “Error” and they remain at around 23%.

I wonder if anyone else is having these problem because I am trying with the different configurations and I always get the same problem.

Just in case you want to check it, find here attach the link to my project:
https://www.simscale.com/workbench?publiclink=770de0c4-e321-4e14-b6cb-dac8baf1d2d5

Greetings.


#18

@Ovi , this is a simple fix. Whenever you have that what you need to do is go to simulation control and increase the maximum run time. I usually have it around 6K but you have to be careful because if it is obvious that your simulation will not converge and you leave it running you are wasting computation time.

Regards,


#19

Hello @jousefm,

I’ve tried to sum up the details from few resources :wink:

  1. The Smooth solver uses a smoother to get a stable solution, in which we usually specify the number of sweeps that the solver should perform. The standard smooth solver uses the Gauss Seidel algorithm. In case of a symGaussSeidel smoother, it performs one additional sweep which makes it ‘stronger’ and better than GaussSeidel while reaching the tolerance values.

  2. With regard to the bounded Gauss upwind scheme - this includes discretization of a third term within the solution to help maintain boundedness of the solution variable, in our case velocity U, and enhance in better convergence especially for steady state solution.

I hope this clarifies your queries!

Regards,
Sam


#20

Thank you @oscarcorripio again for your helpful advices.
Regads.


#21

Hello guys,

I´ve got this error without any message:

aerospace, aircraft cabin ventilation simulation error

Please find attached below my project link in case your would like to check.

https://www.simscale.com/workbench?publiclink=d0798e4c-38ac-463d-a78e-29557fde3553

Thanks for your help.

Greetings
Alex