Hi Niklas,

firstly, yes, I do have a 'real' wedge. The thing is that I could not get the geometry with a 5° slice in Gambit right (checkMesh would fail) so I was wondering if I could apply the wedge boundaries also on e.g. 20° wedges. Furthermore, openFoam complains when my geometry lies along the y axes, i.e. the plane x-y (i.e. z=0) is the symmetry axis. According to the guide this should be o.k. but apparently there is something wrong.

Regards,
v.p.

Hi all!

Problem solved! When the wedge has only one cell in the tangential direction and the x-y, i.e. z=0, is the symmetry plane everything works fine! With more cells there are some problems.

Thanks for everything!

v.p.

[niklas]

Have you read Table 6.1 in the documentation?

http://www.opencfd.co.uk/openfoam/do...#x30-1600006.2

[mattos]

Hi Guys

Tommaso suggested me to try to use the reactingFoam application (solver) for non-premixed combustion flows. I did look for a tutorial for this application same in my previous openfoam instalations without success. Please, somebody can help me suppling a reactingFoam tutorial test case? I think that many other people will also be glade.

Many tanks in advance

Wladimyr

[hannes]

Hello Wladimyr,

I have modified the dieselFoam-tutorial for creating a reactingFoam-Case. I will send this case to you.

Best regards, Hannes

[mattijs]

Hi Hannes,

if you think this case is generally useful do you want to post it on the wiki (http://openfoamwiki.net/) or here?

Does it have FoamX configuration files with it?

Regards,

Mattijs

[mattos]

Hi Hannes and Mattijs


First of all I would like to send big tanks for Hannes to make it available for me. I just received it and I will work now over

Mattijs, I just wrote for Hannes asking him to give me a green light to make it available in the OpenFoam wiki's site. It will be great pleasure for me, however I think that Hannes is the best person to do it because it is his credit.

Tanks for all.

Regards,

Wladimyr

[hannes]

Hello all,

I just put the case, which I sent to Wladimyr, into the Wiki plus some comments.
FoamX files are not included, since I do not use FoamX.

Regards,
Hannes

[gschaider]

I moved your tutorial to a separate page in the Wiki because

a) it deserves a page on it's own
b) it's easier to reference it (http://openfoamwiki.net/index.php/Tut_reactingFoa m_firstTutorial)
c) I'm so glad that there is a first tutorial page on the Wiki now

(It's still linked from the page with all the tutorials)

[mattos]

Hi Bernhard

For new contributions in wiki page, what we must to do? To edit the contribution as donne by Hannes or put in special place directly and make a link to the contribution such as you did? If this last option is right, please could you guide me how do it?

Regards,

Wladimyr

[mattos]

Hi Guys

I need a help. I'm testing the dieselFoam solver with the aachenBomb tutorial case and I have problems trying to restart it. If I put to run with the controldict such that:

startFrom firstTime;

I have not problem and the case runs. But when I put the case to restart using, for example:

startFrom startTime;

startTime 5e-05;

The solver crashes and the following message apears in the output.

==========================================
.
.
.

Evolving Spray

--> FOAM FATAL ERROR : attempt to use janafThermo<equationofstate> out of temperature range 200 -> 5000; T = 1.46567e+161

From function janafThermo<equationofstate>::checkT(const scalar T) const
in file /home/dm2/henry/OpenFOAM/OpenFOAM-1.2/src/thermophysicalModels/specie/lnInclude/ janafThermoI.H at line 73.

FOAM aborting
======================================

I tested using either binary as ascii writeformat and both does not work. Could somebody help me?

Many tanks in advance

Wladimyr

[gschaider]

@wladimyrs question about the Wiki: I prefer a seperate page (just the way I moved Hannes contribution). That way it is easier for me to maintain the Wiki.

Some guidelines about what should go where and how pages should be named can be found at: http://openfoamwiki.net/index.php/Main_Policy

(Adding a page in the Wiki is quite easy: find the page where you want to link from and add a link there by simply writting the name of the page in double square brackets. If you click on that link and the page doesn't exist you will be redirected to page where xou can edit that page. Pointers to more detailed descriptions of the process can be found at http://openfoamwiki.net/index.php/Help:Editing Feel free to use the TestSide-part of the Wiki if you want to try it out)

[mattos]

Hi Hannes,

and others Neros like me!

I have a small suggestion. In the tutorial case given by Hannes, I changed the thermophysicalProperties file in order to be the more general as possible. I left the Hannes' case in the "hannescase" directory as a child of $FOAM_RUN/tutorials/reactingFoam directory. I think that this way can be more general. Bellow, I copied the 2 lines modified in that file. This was the unique modification that I did in the Hannes' test case. It seems that it works fine. Tank again Hannes for your help.

Regards,

Wladimyr


============================================

CHEMKINFile "$FOAM_TUTORIALS/reactingFoam/hannescase/chemkin/chem.inp";
CHEMKINThermoFile "$FOAM_TUTORIALS/reactingFoam/hannescase/chemkin/therm.dat";

[mattos]

Hi Guys

Excuse me, I'm lying! There are the 2 right lines modified in the thermophysicalProperties files. I changed it to make a test and I did'n check. Now is correct! (I hope!)

Bye,

Wladimyr


CHEMKINFile "$FOAM_RUN/tutorials/reactingFoam/hannescase/chemkin/chem.inp";
CHEMKINThermoFile "$FOAM_RUN/tutorials/reactingFoam/hannescase/chemkin/therm.dat";

[finch]

I downloaded this case from the Wiki, but it crashes with the following message. The only thing I changed was the paths to the files chem.imp and therm.dat. Please let me know if you have any idea what's wrong.

---------- Error Message -----------
Mean and max Courant Numbers = 0.0147348 0.0988445
deltaT = 2.43902e-05
Time = 0.0564878

Solving chemistry


--> FOAM FATAL ERROR : attempt to use janafThermo<equationofstate> out of temperature range 200 -> 5000; T = 5000.06

From function janafThermo<equationofstate>::checkT(const scalar T) const
in file /home/dm2/henry/OpenFOAM/OpenFOAM-1.2/src/thermophysicalModels/specie/lnInclude/ janafThermoI.H at line 73.

FOAM aborting

[gschaider]

I would guess, that your reactions produce too much energy and the simulation is "overheating".

Have you changed anything about chem.inp?

[finch]

No, I did not change anything in the case, except the paths to CHEMKINFile and CHEMKINThermoFile. To make sure, I unpacked the archive again and ran the case. I got exactly the same error. Did Hannes, or anyone else, run the case all the way to completion?

[hannes]

Hello,

I just tried to run the simulation further than I did before and I get the same error as Craig. (I did not notice this error before, because the timestep included was the last one I computed).
It seems as if the large temperatures come from the chemistry solver, because a short time before the error occures the largest temperatures are found in the reaction zone and are far above 4000K.
I do not known if such high flame temperatures for Heptan/Oxygen are reasonable. Perhaps someone else knows?

[niklas]

I've now looked at this setup and I think it is bad.

I made some modifications and it ran fine.
but first though, you are only using 5 species and
one exothermic reaction, which constantly feeds the
high temperature region
with fuel and oxygen and no inert gas, so why shouldnt the temperature keep on increasing.
Reality is another matter...

What I did to get it running was this.
I dont know what the real conditions are so...
Initial conditions, N2 95%, C7H16 5%, temp 1500K

50% N2 in both O2 and C7H16 feed
and lowered the inlet temp to 300K
Then the O2 feed will ignite immediately and produce the pilot flame until the heptane starts to mix with the O2

[niklas]

When you use the chemkin stuff all the species are created using the species section in the chem.inp file.

And in order to solve the transport equation for each
and single every one of these you need to specify
the initial/boundary conditions.
So if you have 100 species you need to define the boundary conditions for a 100 species.
I thought this was a very bad idea since usually you only want to vary fuel/O2/N2 and some EGR components.
Hence, when you start the calculation, any species that does not find a definition of its initial conditions and bc's will look for a default settings file, radically called Ydefault.
It is possible to have default setting of initial conditions, but not of boundary conditions, therefore the Ydefault file is needed.
When you start the calculation and look in the newly created time-directories you will see that every species now has its own file (as it should)

The chem.inp and therm.dat files are compatible with chemkin, I do not know if cantera is that.
However, looking at your error-message it is clear that something is wrong with '1O2' and since there only is one place in the file where that combination of characters exists I would move the '11O2' statement one step to the left.