SimScale CAE Forum

Workshop 2 Session - 1 Homework: Optimization of a wing - Part II


#1

This post is a continuation of Aerospace Workshop 2 Session-1 Homework and it contains the tutorial to setup the simulation for Aircraft wing/blended winglet.

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 is assumed to be Inompressible due to velocities lesser than Mach 0.3. 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

  • Click on the tree entry ‘Topological Entity Sets’. The order of choosing the sets is based on ease of selection.
Symmetry:
  • To create the first set, click the shown surface (boundingBox5) and click on the ‘New from selection’ button to create a set named ‘Symmetry’.

Slip wall:
  • Similarly, select the shown surface (boundingBox6) and create a new set named ‘Slip wall’.

Inlet-Outlet:
  • The faces shown below (boundingBox1, boundingBox2, boundingBox3 and boundingBox4) are selected for defining the ‘Inlet-Outlet’ condition

Wing:
  • The Wing surfaces (solid_0_shell_0_face_0 and solid_0_shell_0_face_1) are selected and named.

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

  • The following values are to be defined for initial conditions.
Pressure:
  • Enter the pressure value 100000 [m2/s2].

Velocity:
  • Enter the velocity values 9.84807753 [m/s], 1.736481776 [m/s] and 0 [m/s] in x, y and z directions respectively.

Turbulent kinetic energy:
  • Enter the k value 0.000375.

Boundary Conditions

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

  • Click on ‘Boundary condition’ and select New.

Inlet-Outlet:
  • Enter the Custom boundary condition with a x, y and z-direction velocities of 68.93654271, 12.155372436 and 0 m/s respectively, and pressure set to Zero gradient. * Select the Inlet-Outlet entity and click Save option.

Symmetry:
  • Next we will create the symmetry condition.
  • Select a Symmetry boundary condition, select the symmetry entity and click Save option.

Slip wall:
  • Create a boundary condition named Slip wall with Type Wall and velocity type Slip.
  • Select the Slip wall entities and click Save option.

Wing:
  • The remaining boundary definition is for the Wing.
  • Create a New boundary condition of type “Wall” and velocity type with No-slip.
  • Select the Wing entity and click Save .

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 : 0.15
U : 0.35
k : 0.35
Omega : 0.35
Number of non-orthogonal correctors : 1
Pressure reference value : 100000

  • The relative tolerances for GAMG pressure solver is changed to 0.005
  • Number of pre-sweeps 1

  • The velocity, turbulent kinetic energy and specific turbulence dissipation solvers are changed to Smooth solver with default settings.

  • The gradient schemes for pressure and velocity are changed to cellLimited Gauss linear type.

  • All the Laplacian schemes are set to Gauss linear limited corrected.

  • Set the divergence schemes to bounded Gauss upwind.

Simulation Control

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

Result Control

  • Result control items help us get the surface, force and moment data out of the simulation.

  • Select Result Control and select New against ‘Forces and moments’.

  • Add the forces and moments type, with a density value of 1.2 kg/m3. Select the Wing ‘face set’ and click the Save button.

  • Add another ‘Surface data’ under result control items.

  • Select the Dimensionless wall distance (y+) and click the Save button.

Create New Run
  • Click on Simulation runs to create a new run and start the simulation.

  • Note that multiple simulation runs can be started in parallel. Hence you can start setting up the next case.

Aircraft blended winglet

For the next set of simulations Aircraft blended winglet, duplicate the current simulation and follow these steps.

  • Click Domain from the tree and select the new mesh Aircraft blended winglet mesh.

  • The tree now looks as follows.

Create Topological Entity Sets

  • Go to Topological entity sets and create similar sets for inlet-outlet, symmetry, slip wall and winglet for the new mesh.
Symmetry:
  • Select the face as shown (boundingBox5) and click New from selection, naming it as Symmetry.

  • Now select this entity which is created and click Hide selection button.

  • Select the face shown (boundingBox6) and name it as Slip wall. Similarly hide this face after naming it.

  • Now choose the 4 walls (boundingBox1, boundingBox2, boundingBox3 and boundingBox4), and create an entity called Inlet-Outlet. Hide this selection as well.

  • Now right click in the viewer and click Select all, and name this entity as Winglet**.

  • Assign the material air to the new region, similar to that of the previous setup.

  • Assign the boundary conditions to the new topological entities created.

  • The simulation takes between 160 to 200 mins to finish.

Post-processing

  • Once the simulation is over switch to obtain the results by clicking on Post-processor tab on the top. Select the solution field (Run 1 in this case). Note that the solution field by default includes the internal mesh.

  • Surface contours needs to be plotted. In order to do this, right click on the solution field and select Add result to viewer. This by default introduces another internal mesh.

Surface contours:

  • Go to Mesh Regions from the property panel and select all the surface walls of the wings, i.e. solid_0_shell_0_face_0 and solid_0_shell_0_face_1. Select the Tick to apply.

  • Now select field as pressure p [point-data].

Slice Filter (2D):

  • Select the internal mesh solution field ‘Run 1’ and click Add filter option to select Slice. We include a slice to the domain in order to see the pressure contour.

  • Apply the following slice properties and click the ‘Tick’ icon to apply.
    Slice type - Plane
    Origin - default values (30, 0, 0.002)
    Normal - (0, 0, 1)

  • Select the pressure data p [point data]. Click on the ‘Color bar’ below the selection panel to view the ‘legend’ bar and re-scale to auto range.

  • Change the field to U [point-data] to see the velocity contour.

Streamlines:

  • Hide the slice by clicking the small round next to the slice. Select the internal mesh solution field and click Add filter, for inserting 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 point source stream tracer (Please leave the other properties with default values).

Vectors - U
Maximum Streamline Length - 240
Seed Type - Point Source
Center - (0, -0.5, 16)
Number of points - 150
Radius - 0.5

  • Click the ‘Tick’ icon to apply.

  • Similarly perform the post-processing of the other configuration and compare!


Workshop 2 Session 1 Homework: Optimization of a wing - Part I Meshing
#2

#3

#4

Hello,

During the simulation explication, during the following paragraph, the picture beneath have different values. Which values should we use, also the omega values are never specified, hence should we leave the default values?

Inlet-Outlet:

Enter the Custom boundary condition with a x, y and z-direction velocities of 9.84807753, 1.736481776 and 0 m/s respectively, and pressure set to Zero gradient. * Select the Inlet-Outlet entity and click Save option.

Thanks for your time, great course!


#5

Hello @afemat,

Thanks for pointing this out! :slight_smile: That was a typo and I’ve updated the values now. Please use the values shown in the image.
And yes! Default values can be maintained for omega.

Regards,
Sam


#6

Hello,

At first I was having some problems with the simulation, then I realized I had selected “outlet-inlet” instead of “inlet-outlet”.
Now I have a successful simulation but i can’t view my results, when I select “solutions fields” it keeps loading and never show the results. Can it be a problem with internet connection, browser or my computer?

Thanks,
Henrique


#7

@sjesu_rajendra . I have tried to run the cases but it turns out I am not allowed to have a maximum run time of more than 9999 seconds. This is not enough to run a whole 2000 timesteps. Actually it didn’t even run 1000 timesteps (based on 9000s). I thought that at the end of the simulation it would automatically save the last timestep but it hasn’t. As a result I now need to run the simulation again.


#8

Give a try again now, I had the same issue but it’s already working… Be patient, is 1GB per simulation of data that needs to load every time we do a change


#9

Hello @rapetrei,

I had a look into our system and see that you have subscribed for a free premium test account, which has only 200 core hours (CH) for computation. You have already exceeded this CH quota. If you prefer, I can switch your account to the community account and you can continue your simulations with up to free 3000 CH usage. Please let me know so that I can proceed with the same.

Regards,
Sam


#10

@sjesu_rajendra yes please. I didn’t know which type of account I should be signing for. Also would it be possible to change the username from “rapetrei” to “rmapetrei” (for obvious reasons). It was automatically generated and didn’t notice when I confirmed it as it is similar to my email address.


#11

Hi @rapetrei did switching to the community account work for you?

I currently have the community account (with the 3000 core hours) and it cancels the simulation after 63 - 64 minutes due to exceeding the computation time.

Thanks!


#12

@JeremyG still waiting for them to change my account subscription.


#13

@rapetrei,

Unfortunately it is not possible to change the username at the moment. The username acts as a link to all your forum activities and projects, which becomes inaccessible once the username is changed.

With regard to your account downgrade, I have already changed your account type. But I’m not sure if the switch is done yet - if it’s not updated please wait until tomorrow.

Sam


#14

Hello @JeremyG,

Please change the Maximum runtime setting under Simulation control and re-run the simulation. When defining this make sure you give enough time for the simulation to complete. This setting acts like a safety switch :wink: in order to limit your simulation that it does not run forever, burning down all your core hours.

Sam


#15

I am having a weird problem, mesh with no winglet completed with no problems however, with winglet is stuck as in “Queued for computing” for almost a day now, I tried deleting it, didn’t work and then I duplicated that and ran it again and shows me ‘error’, with no description of the error.

Also, for simulation part, it took me close to 14hrs is it alright? considering 32 cores were used.


#16

Hey @rahulsharma_94,

This is not alright :worried:… I don’t see the error run in your project. Is it already deleted? Could you please let me know if you tried to run the case again?

Sam


#17

I made two cases for that just to see if I did something wrong, as you can see in the first image it still shows ‘Queued for computation’ and other variant shows error.


#18

Hello @rahulsharma_94,

There is some issue with the mesher and our Product Engineers are looking into it now. I will let you know when the problem is resolved. Please try mesh generation after that.

Regards,
Sam


#19

Hello @rahulsharma_94 and any other participants who have the mesh issue,

I just got some information from our Product Engineer. It seems to be a bug between OpenFOAM and one of the 3rd party libraries, which happens during parallel computing. The issue is still not solved since the reason is non-deterministic at the moment. But we have a workaround for now - if it is necessary to run the mesh at 32 cores please tweak the settings a little bit (say change the bounding box dimension by a very small value or the number of cells along any direction by a very small number, say 1) and re-run the case.

A better solution would be to run it in reduced cores, say 16. This should help for the time being. Meanwhile we are working on it to eliminate this problem completely.

Sam


#20

Hi there,
I’m on the simulation run stage however I have encountered a problem :

The maximum run time of this job would exceed your computation quota.
You can try to adjust the settings under ‘Simulation Control’ and to create a new run.<<

any help on what to do next
Thanks