simpleFoam always diverges
 

Dear CFD-Community,

i am having very big problems with the simpleFoam solver.

The aim is to simulate the airflow around a streamlined body and get to know about the drag coefficient. I am using a cylindric computational space around this body...

But always - after few timeSteps, the calculation gives out abnormal results and little time later, it will collapse :(

I posted also some screenshots, that will show the velocity behavior...

Could someone help me?

Thank you very much in advance

RugbyGandalf

Hi,

post your case files (without grid), otherwise I can't help you

Regards,
Christian

Dear Christian,

thank you very much for your reply...

I will upload the case files without the start velocity field, because this would be to much data for 370k cells...

this is my 0/ start directory

i am calculating with kOmegaSST, as you may see in RASProperties, detached here:

And i also posted the system/ folder...

Would be grateful, if you are able to find the mistake...

Greetings

Rugby

PS: needed to transform them into txt for upload :(

Got the idea to zip it:

so once again :)

Well,

The boundary files could not be understood, not in English you know.

Anyways, here are few suggestions:

1. Under-relaxations : p 0.15 , U 0.5
2. divSchemes : Use upwind for 'U'

You could switch to higher order schemes later as the solution stablilizes....

Hi,

have to tried to use a different turbulence model (e.g. k epsilon) to see if the problem is related to the kOmegaSST model? The kOmegaSST model is a bit difficult to use (at least from what I heard).

Is the slip BC really correct? I'm not familiar with this BC.

Try the fixedMeanValue BC (openfoam 1.6 ext) for the pressure outlet.

What type of grid to you use. Have you checked to quality? Maybe try to increase the nNonOrthogonalCorrectors.

Also, try faceLimited grad schemes.


Regards,
Christian

Hello, RugbyGandalf,


does your case run with turbulence switched off (i.e. laminar)? If so, it's most likely the turbulence model causing trouble.

Can we have the results of a checkMesh run through your case?

I have a problem with the inlet BCs for the turbulent quantities, i.e. k and omega. Could you explain, why you use these values? What's troubling me: at the inlet you have set a very low value for k (0.083 m²/s²) while the velocity is quite high there (40.57 m/s). This results in a very low turbulence intensity at the inlet:



I'm guessing you're imposing a low turbulence inlet with this value. But you also have a very low value of omega at the inlet (0.814 1/s), which results in a rather big eddy viscosity ratio:



This means the turbulence viscosity is almost 5 orders of magnitude bigger than the molecular viscosity! I don't think this is physically correct and I also think this may be giving the turbulence model a hard time.

Please read this article if you'd like to redo your turbulence boundary conditions: http://www.cfd-online.com/Wiki/Turbu...ary_conditions


Greetings,
Felix.

Rugby,

there are 3 issues, here listed according to their importance:

1) Never ever initialize k, omega (or epsilon) with fixedValue 0 on solid bodies. Therewith you provoke a division by 0. For high reynolds models like 'kOmegaSST' use zeroGradient on your body.

2) The tolerance for p should not be greater than for U, k, omega (,epsilon).

3) I prefer to initialize with (0 0 0) as internalField for U.

Respecting 1) should tremendously improve your case!

Hello again and thank you very much for your hints...

the calculation is still not correct, even after changing the parameters :(

i will upload the actual case...

i have done the following:

- set relaxion factors for p to 0.15 and for U to 0.3
- using Gauss upwind for U divSchemes
- faceLimited Gauss linear 1 GradSchemes
- used english expressions for BC / Grid

fixedMeanValue BC is not available for OpenFOAM 1.7.1

I am also posting the checkMesh Result

@ lord_kossity: i am trying with your hints, after posting this !!!
@ Felix, you were right, i mixed the files of another case, accidentally - i got the (it seems to me) right values for k and omega now... sorry for that - unfortunately it will not work with them neither :(

Thank you very much so far

Greetings

RugbyGandalf

k file in 0/ directory has been updated - case_act.zip

actual case with updated values for k - sorry for confusion

Hello, RugbyGandalf,


your checkMesh looks OK, so there probably isn't a problem related to the mesh.

Have you already tried running the case without turbulence modeling?

Thanks for posting your updated parameters, but now the eddy viscosity ratio is twice as high as it was before! Do you really want to have values for the eddy viscosity at the inlet of the order of 0.1 m²/s? This is an oil-like viscosity and judging from your transportProperties dictionairy you're trying to simulate an air flow case, am I right?

Please try a value of 30000 for omega at the inlet and the initial field. This leads to a much, much lower eddy viscosity and hopefully the solver is able to handle this. Unless of course it is your intention to have so big eddy viscosity values at the inlet.

The fixedValue 0 settings for omega and k shouldn't pose a problem - if so, the simulation would've already crashed before finishing even one iteration.


Greetings,
Felix.

Dear Felix, thank you very much for your reply...

now i got the case working - with the parameters of the new postet cas_working.zip

i also posted two screenshots - showing the velocity and the pressure! Both look correct for the first view...

I am wondering about you high value suggestion for omega - i calculated omega and k from the following formulars:

k = 0.5*(Ux')^2
Ux' = TU*Ux where TU for our wind tunnel is 0.02 and Ux is the main stream velocity
so i got:
k = 0.5 (0.02 * 40.57)^2 = 0.32918

for epsilon:

epsilon = (Cmu ^ 0.75 * k ^ 1.5)/l where Cmu is 0.09 and l is 0.65 for our wind tunnel
epsilon = 0.0477

so i will get for omega = epsilon / (Cmu * k) = 1.6124

i got these formulars from my projekt - supervisor...

I also calculated those values with the formulas from your link - the values are a little bit different, but overall in the same range...

As i mentioned: the calculation works now - but i will get the wrong drag-coefficient
it has to be around 0.06 - and i get a value of 1.7 - 1.9

Do you have any idea, what causes those problems?

Greetings

Martin

Hi Martin,

I am relative new to CFD and OpenFOAM, but maybe it helps, if you was using inlet conditions for kOmegaSST as proposed in Menter (1994): Two-Equation Eddy-Viscosity Turbulence Models for Engineering Applications. This way you will get quite low turbulence at the inlet, but the turbulent viscosity ratio is not that high.

Looking forward to your progresses.

Gerard

Hello, Martin,


could you post a contour plot of the eddy viscosity (nut) and the other turbulent quantities with numerical scales, please? Might give a better idea about the much too high drag coefficient.

And by the way: I still can't reproduce your turbulence dissipation values. You wrote l is 0.65m for your wind tunnel. What's the dimension of your model and wind tunnel? Have a read here: http://www.cfd-online.com/Wiki/Turbulent_length_scale


Greetings,
Felix.

I posted my screenshots of omega, k and nut here...

omega and k seem to have the same value for the whole field, except near the body, that is why i zoomed it...

The dimension are the following:

the streamlined body has a length of 0.2 m, It's diameter at the biggest position is 0.078 m.
The wind tunnel is rectangular with a length of 1 m a side. The experimental values have not been token inside, but as you can see on the plan - screenshot (sorry for the bad painting quality) on a gap of this tunnel.

I am going through your given lecture links now and try to get to know how to calculate the right values...

If you have any new hints, please let me know ;)

Regards,

RugbyGandalf

Hello, Martin,


judging from your nut-plot, the eddy viscosity is way too high (like I suspected). Please select a value for the turbulent length scale L, which is much more reasonable. 0.65m is clearly too high. Please read the links I posted above to better understand this property of turbulent flow.

There's another way to calculate omega: with the eddy viscosity ratio (nut/nu) you can specify omega at the inlet. The eddy viscosity ratio for wind tunnel experiments should be in the order of 1.


Greetings,
Felix.

Dear Felix,

i tried various values for k and omega in different combinations...

i will open a new thread for the drag coefficient problem, because the first problem - simpleFoam always diverges - has been solved with all your grateful help - thank you all very much...

By the way, at least the calculation also worked with a starting velocity in the hole field.
I set down the timeStep in controlDict to a very small value manage the CourantNumber request.

Thank you very much

Greetings,

Martin

Would you happen to have a reference paper for that statement?

Hi
 

Dear RugbyGandalf

can you upload your mesh file ?
Greetings,

Martin[/QUOTE]

Hi RugbyGandalf,

I made an investigation on NACA 0012 airfoil in low and high mach number flows. One of the things that I found to be very important is the windtunnel investigation itself. Check if the results have been corrected somehow for wall interference and all these things. I found it very helpful to get the pressure distribution right first and the look for drag.
To me your domain looks much too small. I got good results with at least 5 to 10 chord lengths distance between the airfoil and any boundary at 0° angle of attack. For 15° angle of attack I needed 22 chord lengths.
Personally I would use the slip boundary condition on the cylinder for velocity, but the zeroGradient condition instead. With slip you disable flow through the walls, which seems reasonable at first glance. However you don't really know (or you need a detailed report) if the wind tunnel is slotted of the test section is even open. Therefore you impose a constraint, which is not present in the wind tunnel.
My simulation showed a drag coefficient, which over estimated drag by 40%. I suppose better is possible. So don't give up.

Regards