CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM (http://www.cfd-online.com/Forums/openfoam/)
-   -   ChtMuliRegionFoam-Case (OF 1.6 Tutorial-case -> OF 1.5) (http://www.cfd-online.com/Forums/openfoam/69166-chtmuliregionfoam-case-1-6-tutorial-case-1-5-a.html)

suitup October 14, 2009 04:30

ChtMuliRegionFoam-Case (OF 1.6 Tutorial-case -> OF 1.5)
 
Dear Foamer,

I have seen that in 1.6 there is a new tutorial-case for the ChtMuliRegionFoam-Solver. Would it work if I run theis case in 1.5?

The solver already exist in 1.5 and I dont wanna install 1.6 cause i have to upgrade ubuntu 8.04 and so on...

Or have you an test-case you can upload here?

Thank you very much in advance.

LarsPT October 14, 2009 10:12

The case won't work with OpenFOAM-1.6 unless you change some things that have changed between 1.5 and 1.6:

1. pd has been substituted by p. Therefore change the filename in the 0 directory and replace buoyantPressure BC by zeroGradient BC without setting any value.

2. environmentalProperties are now called g. So you have to change the filename and specify g in there. Actually you can copy the environmentalProperties of another OF-1.5 tutorial case regarding the direction of g.

3. The solver control syntax has changed. Look at the OF-1.6 case and compare it to any other OF-1.5 case. You will find the difference soon. It's not difficult to change for use with OF-1.5.

I think this is it. Good luck!
Best regards!
Lars

suitup October 16, 2009 09:58

Thank you for your tips, I try it out, but nevertheless I should mabye install the latest version.

I dont wanna start a new topic, so I hijack this one.

Can I install OF 1.6 on ubuntu 8.04 or would there be some issues?

LarsPT October 17, 2009 03:23

I'm not sure about this because personally I use OpenSUSE 11.1. However,
as ubuntu 8.04 use Qt 4.3.4 as default version it should work concerning the
OpenFOAM installation readme.

Best regards
Lars

ronaldo October 26, 2009 04:14

1 Attachment(s)
Quote:

Originally Posted by LarsPT (Post 233001)
I'm not sure about this because personally I use OpenSUSE 11.1. However,
as ubuntu 8.04 use Qt 4.3.4 as default version it should work concerning the
OpenFOAM installation readme.

Best regards
Lars


Hi LarsTP,

i have tried to run the simulation and have the following error message "s. attachment". Could you tell me please what this means?

Thank you so much! you are the best

LarsPT October 26, 2009 04:33

Hi Ronaldo,

thanks for your commendation even it's a bit exaggerated! ;)
The error message indicates an sigFpe error which means that there is a unallowed math operation, e.g. division by 0.
Check your inital conditions whether you have set a value to 0. Often the k-epsilon values a set to 0 due to laminar flow which leads to the error message. Actually they can be set to any value when laminar flow is choosen in the turbulence settings. Another problem might be too small time steps in the controlDict. As the time step is evaluated by the Courant number set a value of maybe 0.001.

Best regards
Lars

ronaldo October 26, 2009 07:34

Thank you for your reply LarsPT,
(I had set "epsilon" to 0 in the 0.001 folder)

it works! I will send a messange later to inform you how the results look like.
IŽm so happy!!!

ronaldo October 28, 2009 04:14

Hi LarsPT,

i donŽt know what to do right now! nothing happend on the solid surface "no heat Transfert"

I have the next folder " 0.051 because i set the writeInterval to 0.05" and i run foamToVTK -region [region].

"It is too earlier to see something?"
I have set the BCs at the region interfaces as follows:

solidWallMixedTemperatueCoupled
neig... T;
K K;
value 273,15;

please an idea! what should i change or do!

Thank you in advance

LarsPT October 28, 2009 12:14

Yes, it might be to early to see a difference. Of course it depends on the thermal diffusivity of the fin and the temperature difference as driving force.

Did you abort the simulation at this point or do you have such a fine mesh that you only have the first time step for now? If yes I would decrease the mesh resolution to make sure that the case is set up properly and finally increase the mesh resolution.

Best regards
Lars

ronaldo October 29, 2009 07:42

Hi LarsPT,

yes i have a very fine mesh so that i only have the firs time step for now!

OK i Žll decrease the mesh resolution and try again ( IŽll inform you later).

Any other ideas please!

Tank you in advance

ronaldo November 1, 2009 05:14

Quote:

Originally Posted by LarsPT (Post 234372)
Yes, it might be to early to see a difference. Of course it depends on the thermal diffusivity of the fin and the temperature difference as driving force.

Did you abort the simulation at this point or do you have such a fine mesh that you only have the first time step for now? If yes I would decrease the mesh resolution to make sure that the case is set up properly and finally increase the mesh resolution.

Best regards
Lars


I decrease the mesh resolution, but nothing happens anyway!
Please any other idea!

LarsPT November 3, 2009 03:32

Hm, I thought for possible reasons for quite a while now but I don't have any new ideas conceirning OpenFOAM. Pherhaps the temperature difference is to small and therefore the heat conduction will take a lot of time.
Sorry, that's the only thing that comes to my mind.

Good luck!
Lars

ronaldo November 4, 2009 08:57

Quote:

Originally Posted by LarsPT (Post 234926)
Hm, I thought for possible reasons for quite a while now but I don't have any new ideas conceirning OpenFOAM. Pherhaps the temperature difference is to small and therefore the heat conduction will take a lot of time.
Sorry, that's the only thing that comes to my mind.

Good luck!
Lars


Ha Ha Ha!!!!!!! It woks Lars!!!!!!!!!!!!!!!!!!!

i think the BCs at the region Interfaces were not set properly.Futhermore it was to early.
I have to be patient because of my mesh resolution "too fine". I' ll post tomorrow some Screenshots here.

Thank Thank so much!!!!!!!!!!

kawuppdich November 11, 2009 08:10

has anyone calculated with the chtMRF solver in parallel in of15
i got it under 1.6 but i dont know how to decompose the case in 1.5 :confused:

LarsPT November 11, 2009 13:30

I think there is no difference in decomposing a mesh between OF1.5 and OF1.6.

decomposePar -region <regionName> should work properly.
But make sure to create a subfolder for every region in the system directory which contains the decomposeParDict, e.g.
system/<regionName>/decomposeParDict.

Best regards
Lars

kawuppdich November 11, 2009 13:43

Hi LarsPT
when i try it, of15 says it does not know option -region, and when i try with only typing decomposePar,I miss the 0.001 Folder in the processor Folder
same in of1.5-dev


All times are GMT -4. The time now is 09:15.