Compressible flow over two-dimensional bump geometry
 

Hello Forum regulars and guests,

I have recently started working with a 2D geometry consisting of a bump on a wall, a defined inlet and outlet and symmetry conditions on the rest of the exterior boundaries. This is described in detailed within the images attached. This is a benchmark study from NASA and I would like to use it as a reference for code verification. (For Details - http://turbmodels.larc.nasa.gov/bump.html)

I am looking for suggestions to implement the boundary conditions required, to match the reference results. I am trying to obtain steady state solutions using an ideal-gas model, with gravitational acceleration in -y axis. The current boundary conditions including the pressure outlet and inlet have an operating pressure of 101 325 Pa with a gauge pressure set to (101 325 x 0.02828) Pa. This pressure gradient results in a velocity of 69.7 m/s which satisfies the M=0.2 condition. I currently have the energy equation turned off, since I am working through the preliminary stages of the simulation setup. I have received several warnings and recommendations when I clicked Check Setup before commencing with the solver iterations, as shown in the image.

All the convergence criteria for the residuals were defined as 1e-6 however, the continuity simply remains at 1e-2 despite the large number of iterations performed. I tried changing the momentum relaxation factor from 0.8 to 0.5 however, this only had a minimal effect.

Please help me implement the boundary conditions outlined in the first two images and also provide some guidance to improve the absolute continuity residuals. I look forward to your comments.

Here are some images showing the Pressure inlet settings and also the warnings received when using the Check Case feature prior to solving.

Please help me understand the messages and share some suggestions to correctly model this.

Hello everyone,

I am surprised by the lack of any comments on this thread however, for those who are still interested I will post the results here. I have a comparison PDF file and some screenshots of the contour plots. Please provide any guidance or suggestions for improvements. I have not been able to accurately model the temperature boundary conditions and incorporate the energy equations yet however, I am not sure that is causing the difference in the Cf dataset.

All educational comments are welcome.

Hey CFD Online Members,

Hope you are all going well with your individual goals and projects. I am still working with the above geometry and the Cf values are significantly different to the benchmark dataset. The Cp values have much lower errors and this has been a consistent trend for more than 4 different simulation cases.

I am trying to find root causes for this discrepancy and thought about many different sources of errors. Is it possibly due to the 'bump' being a no-slip shear wall and the wall immediately ahead of it specified as zero-shear? It may be having some problems at the transition as the free-stream velocity strikes the edge of the bump profile.

I have also observed that the continuity residuals are not falling below 10^-2 level and this remains unchanged for both transient and steady-state flow simulations. Does this mean that there is an imbalance of mass continuity across the domain and could this be causing the Cf values to vary greatly?

I have attached an image and I look forward to your comments regarding the source of the large Cf errors and some fundamental concepts related to the continuity residuals.

Did you try a "real" symmetry boundary condition instead of a zero shear wall in front of the bump?
They are not equivalent when it comes to turbulent quantities.

And wouldnt it make sense to use a free stream boundary condition at the inlet?

Hi Crank-Shaft,
I would do the following:

--> first of all check your yplus value that should be less than one if you don't use any wall function, this should influence your cf values.
--> then try to do this computation case with density based solver i.e. compressible mode as you are using currently the incompressible solver. This might help too, as it is stated on the main page of this test case that the computations have been carried out using compressible solver.
--> please try to use appropriate boundary conditions.

hope this helps.

best regards and good luck.

You have no pressure gradient from inlet to outlet ! :eek:

Set inlet pressure to 104190.471 pa , outlet to 101325 pa and operating pressure to 0 pa.

You can also try with velocity inlet.


How slip wall differs from symmetry when calculating turbulent quantities?

PS. Are you sure about geometry and mesh? Did you try the solution on meshes available on website...

At walls with zero shear stress, wall-functions for the turbulent quantities are applied anyway.
This is not the case for symmetry boundary conditions.

The effect can be seen e.g. in a 2D channel, where you set one of the walls to symmetry and the other one to zero shear stress wall.