[Time4Tea]

Hi. I've just attempted my first 'serious' simulation in OpenFOAM and thought I would post some images, with some questions and comments that I have.


The model is a 3D half-symmetric model of a control valve. I have done a lot of simulations of these in FLUENT over the past couple of years, so I am comparing the results in Foam to what I usually get in FLUENT. The flow is incompressible water, with a lot of separation and mixing, so I have used the simpleFoam solver with k-epsilon turbulence model. You can see from the images that I created a polyhedral mesh in FLUENT and then imported it to OF. It has 10 inflation layers. For boundary conditions, I used totalPressure at the inlet of 517 kPa and static pressure at the outlet of 345 kPa. I used the nutkWallFunction on the walls.


I had a little bit of trouble at first with the field initialization. Normally in FLUENT I would use the hybrid initialization method, which actually solves some simplified equations to give an initial flow field. However, it seems that OF doesn't have this? Anyway, I eventually had some success with setting the initial velocity everywhere to 0 and initializing the pressure everywhere to the outlet pressure.



In terms of the solution, it converged quite nicely and seemed to settle to a very similar overall volumetric flow rate that I had achieved in FLUENT. However, the k and epsilon values in some areas seemed very high (as can be seen in the contour plots - max. k ~50, max. epsilon ~400,000), which I didn't get in FLUENT. However, these high values didn't seem to be having a huge effect on the overall volumetric flow result and also the turbulence equations seemed quite stable. The residuals for the turbulence equations were quite low (< 10^-4).


So, it seems that the solution was converged with those high k, epsilon values. In that case, I would think the problem must be an inaccuracy in the model equations that I am using - perhaps the wall function or the yplus values are not appropriate?


I tried to check the wall yplus; however, I got the following error

/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  6
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
Build  : 6
Exec   : postProcess -time 25 -func yPlus
Date   : Jul 07 2019
Time   : 06:54:13
Host   : ***
PID    : ***
I/O    : uncollated
Case   : ***
nProcs : 1
fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 10)
allowSystemOperations : Allowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 25

Time = 25

Reading fields:

Executing functionObjects


--> FOAM FATAL ERROR: 
Unable to find turbulence model in the database

    From function bool Foam::functionObjects::yPlus::execute()
    in file yPlus/yPlus.C at line 185.

FOAM exiting

Does anyone know how I can resolve this?


Another couple of questions that I have:


1) Is there any equivalent in OF to the pressure-based coupled solver in FLUENT? I often use that for these types of internal flow problems and find that it tends to converge faster than the segregated algorithms.


2) I really like Paraview! It seems better for postprocessing than either the built-in capabilities in FLUENT or CFD-Post. Does anyone know if it is possible to export FLUENT data into Paraview?


Thanks in advance

[Tobi]

Hi,

I just read your error message and can give you the following info:

yourSolver -postProcess -time 25 -func yPlus

[Time4Tea]

@Tobi: ah, thanks! That worked.


It seems curious that it is necessary to invoke the solver though. I would have thought the postprocessing would be done on the result data files, independent of whatever solver was used to generate them.

[hxaxtma]

It seems curious that it is necessary to invoke the solver though.

yPlus needs the value of viscosity which is retrieved by invoking solver. Same for wallShearstress.

Is there any equivalent in OF to the pressure-based coupled solver in FLUENT?

Have a look at foam-extended

it is possible to export FLUENT data into Paraview

If Fluent can export the data in Ensight format you can open the data in paraview

[Time4Tea]

@hxaxtma: thanks for your helpful advice.

[Time4Tea]

So, does anyone have any idea what might be causing the unrealistic k/epsilon numbers? For the wall boundary conditions, I am using nutkWallFunction in the 0/nut file; kqRWallFunction in the 0/k file; and epsilonWallFunction in the 0/epsilon file.


I also tried running the same case with the kOmegaSST turbulence model, thinking it should be less sensitive to wall y+ than k-epsilon; however, the k/omega solutions explode within a few iterations. There, I again used nutkWallFunction in 0/nut; kqRWallFunction in 0/k; and omegaWallFunction in 0/omega.

[misospider]

As k-epsilon works kwSST doesn't work, I think there could be two main possible reasons.

1. Mesh (especially for boundary layer)
2. BCs

Because kepsilon model is assuming fully developed flow, usually y+ range is 30-100.
kwSST usually requires y+ range from 5 to 30. So, kwSST is more sensitive to boundary layer mesh.

And I wonder what initial GUESS values for k ,e and w you used.

It is better to use values from calculator, which are available on this site.

https://www.cfd-online.com/Wiki/Turb...ary_conditions

https://www.cfd-online.com/Tools/turbulence.php