Defining custom Cp library under 2.2.x
 

I'm trying to update my code to run with 2.2.x and part of doing this involves porting over our Cp and viscosity libraries. Prior to this, declaring a new library for the various thermotypes involved adding the thermotype to the list of thermotypes in the *thermos.C files (like psiThermos.C). For example:

This seems to not be sufficient in the new version. With the new ThemoType definitions there seems to be an additional place to declare the new library name.... what leads me to believe this is at runtime my code gives the following error:

You'll notice that the place where "myJanaf" should appear as a valid choice is blank shoving all the columns over to the side. I interpret this as the runtime selection table is reading the thermotypes from psiThermos.C and picking out the valid thermotypes but when it gets to "myJanafThermo" it can't recognize it and it skips over it.

Does anyone know where this magic happens? Or what I'm missing? I've spent far more time than any one person should trying to find this and I can't imagine I'm alone in having this issue.

Also related is that upon execution the code spews the following:

for what appears to be all of the runTime selection tables... or something, I don't completely understand whats going on there but it started happening as I added my thermotype so I imagine (hope) both issues resolve themselves together as soon as I find the piece of the puzzle I'm missing.

For some reason 90% of the time I post something here I find the answer 5 minutes later. It looks like I was missing the following in my janaf code:

I guess stopping for a minute to put a problem to "paper" is enough to jar the brain into a different and often more productive thinking state :p Although I'm still getting the duplicate entry stuff at the start of my code... for reasons unknown.

Dear ChrisA:
I have some problem like you.I want use the thermo type as the following:

thermoType
{
type hePsiThermo;
mixture reactingMixture;
transport sutherland;
thermo janaf;
energy absoluteEnthalpy;
equationOfState perfectGas;
specie specie;
}
but class hePsiThermo only have "sensibleEnthalpy" insteadingof "absoluteEnthalpy".In 2.2.1,only when I use heheuPsiThermo,can I use "absoluteEnthalpy".So I have to according to class heheuPsiThermo to add "absoluteEnthalpy" in class hePsiThermo .However,when I run my case,the error showed me that there no change with "Valid psiThermo types ".In other word ,my modifies did not work.the file I modified is "thermophysicalModels/reactionThermo/psiReactionThermos.C"I just put the following code:
makeReactionThermo
(
PsiThermo,
PsiReactionThermo,
hePsiThermo,
reactingMixture,
sutherland,
absoluteEnthalpy,
janafThermo,
perfectGas,
specie;
) and #include "absoluteEntalpy.H" to psiReactionThermos.C.As you know ,it did not work.could you tell me how to modify psiReactionThermos.C to make my difined thermo type :
{
type hePsiThermo;
mixture reactingMixture;
transport sutherland;
thermo janaf;
energy absoluteEnthalpy;
equationOfState perfectGas;
specie specie;
}to be useful?
I think you can tell me something about my problem.With your post,abviously,you know of2.2.1 better then me.
Please!

OK here is how you enable e.g. the absolute enthalpy in your solver. The coding involved is very simple, once you know what to do. :)
1. Create a new library that assembles the necessary bits:
I attached a zip archive with the necessary code to include the standard OpenFOAM absolute enthalpy thermo, but this can be extended easily to own implementations of e.g. Cp or viscosity as well.

2. Link your solver against that new library:
I assume you know how to link your solver against new libraries, at least there should be some tutorial/wiki somewhere.

@ChrisA: Just out of curiosity, which new "Cp and viscosity libraries" do you wanna implement?

-Armin

That looks marvelously simple, I knew there had to be an easy way to add things to the run time selection table... I just never thought of compiling a new library with them in there. (The run time selection stuff is still largely a mystery to me) I'll give it a try when I get a chance, thank you for posting that.

With regards to the libraries I want to implement, the Cp one is simply a higher order polynomial fit than what JanaF uses. I'm fitting a polynomial to Cp for temperatures between 50K and 500K and an extra coefficient makes the fit much better. (rather than fitting -everything- using the polynomial thermotypes). The viscosity model is a kinetic theory based viscosity model... however that is less important as I would need to change how viscosity is mixed at present... So mostly this is so I can have an extra coefficient on the end of my JanaFesq Cp polynomial >.>.

Dear dkxls:
Thank you very much for you reply and your zip archive !But I have some thing can not understang.Would you tell me some explainasions?
1.According your new library myThernmo,There should be only myThermos.C,myThermoTypes.H,and file of "make" in myThermos.What do other file work in your myThernmo?
2.I delete other file leaving myThermos.C,myThermoTypes.H,files and options in "make".I don not chang any codes and use "wmake "with myThernmo.Then,I add "libs("myThermos.so");" in the controlDict of my case.when I run my case,it gives me error:
From function dlopen(const fileName&,const bool)
in file POSIX.C at line 1179
dlopen errer:myThermos.so:can notopenshared object file:Nosuch file or diretory
I have not linked solver against new libraries before.please give a guide to define my thermotype:
thermoType
{
type hePsiThermo;
mixture reactingMixture;
transport sutherland;
thermo janaf;
energy absoluteEnthalpy;
equationOfState perfectGas;
specie specie;
}in your mythermo.I think it is easy to give me advise for you.please,please!

Dear dkxls:
I can link solver against new libraries.I successed to build myThermos.so,and I add the codes:libs("libThermos.so") in the start of "controlDict".Then I run my case,it still give me error:
FOAM Warning :
From function dlOpen(const fileName&, const bool)
in file POSIX.C at line 1179
dlopen error : /home/administrator/OpenFOAM/administrator-2.2.1/platforms/linuxGccDPOpt/lib/libmyThermos.so: undefined symbol: _ZN4Foam15chemistryReaderINS_19sutherlandTransport INS_7species6thermoINS_11janafThermoINS_10perfectG asINS_6specieEEEEENS_16absoluteEnthalpyEEEEEE30dic tionaryConstructorTablePtr_E
--> FOAM Warning :
From function dlLibraryTable::open(const fileName&, const bool)
in file db/dynamicLibrary/dlLibraryTable/dlLibraryTable.C at line 99
could not load "libmyThermos.so".
I think myThermotypes.H may have something wrong,and I also can not understand the codes in your myThermotypes.H .Attachement is my new lirary accoring to your zip archive .Plese take a look on my attachement,and could you give me some advice ?Thanks inadvance!

I have upload my attachement,Attachment 25371please help me to have a look!

@zqlhzx:
After having a closer look at what you actually wanna do, I just can recommend you to use 'sensibleEnthalpy'!

The whole OpenFOAM chemistry implementation is build for sensible enthalpy. In particular, the 'chemistryReader' and 'chemistrySolver' classes are build around sensible enthalpy. Also the top-level solver (e.g. 'chemFoam', 'reactingFoam', ...) are build for sensible enthalpy, as they all include the source term from chemistry in their transport equations.
Now you can "easily" implement all this also for absolute enthalpy, but it involves some more coding than just building the thermodynamics for absolute enthalpy.

If you don't want to change/implement all these things for absolute enthalpy you should just use the sensible enthalpy.

From the thermo-chemistry point of view, it doesn't really matter if you are using absolute or sensible enthalpy, you just have to implement it accordingly - but the end result won't change!

Ah, ok I see. Sounds good! :)

I use for accurate temperature depended viscosity data a polynomial expression (the same as in CHEMKIN):
ln(mu) = sum_i=1^N( a[i] * ln(T)^(i-1) )

I submitted the implementation to OpenFOAM (mantis bug #978), but the developers haven't included it yet. The code, is a straight forward implementation based on the polynomialTransport class and available in the bug report:
http://www.openfoam.org/mantisbt/view.php?id=978

For mixture I use the formulations due to Wilke (viscosity) and Mathur (conductivity), but I haven't contributed that code to OpenFOAM yet.

Dear dkxls:
Do you mean that I also have to change 'chemistryReader' and 'chemistrySolver' classes if I want to build my own thermo type:
thermoType
{
type hePsiThermo;
mixture reactingMixture;
transport sutherland;
thermo janaf;
energy absoluteEnthalpy;
equationOfState perfectGas;
specie specie;}?In other word ,most users who use OF2.2.1 only can use sensibleEnthalpy.I found just XiFoam,PDRFoam and engineFoam use absoluteEnthalpy,but the there solvers are only used in premixed-combustion or partly-premixedcombustion.Compare with old vision,we can use absoluteEnthalpy like in reactingFoam or FireFoam.So I do not think it is not more convenient than old vision when using thermo class to define thermo type in OF2.2.1.Why do OpenFoam change thermo class?I can not understand.

I right now don't know exactly what would be needed to get this also working with absoluteEnthalpy, but at least you need to instantiate the 'chemistrySolver' with absoluteEnthalpy as well (in a similar way as I did with makeReactionThermo).
Also, you need to take care of the source terms in the transport equations!!!

The solvers you mention don't use the chemistry classes, hence no restriction from that side.
So yes, if you want to use a chemistry solver you are limitied to sensibleEnthalpy in standard OpenFOAM.

Well the new thermo classes bring many really good changes and remove a lot of duplicated code! Even if there are right now not that many new features, the infrastructure is now in place to add them!

But why would you anyways want to use absoluteEnthalpy instead of sensibleEnthalpy?
I don't see any reason for this! Seems right now only to be trouble with no advantage whatsoever!
In fact, I do understand why the OpenFOAM developers preferred sensibleEnthalpy over absoluteEnthalpy enthalpy, especially when thinking of sprays and other source terms in the transport equations.
But as already said, it's mainly a matter of taste which which one you choose, the results is the same in the end!

Dear dkxls:
Thanks for your reply again.The solver I use is not developed by myself.It is based on openfoam2.0.1.My teacher ask me to make the solver use in openfoam2.2.1.Although the solver is used to simulation combustion ,but it do not solver transport equation and do not use chemistry solver.Due to the conbustion model the solver uses ,I have to use absoluteEnthalpy,and the original solver(2.0.1) also use absoluteEnthalpy.It is why I use absoluteEnthalpy.
Today,I use your attached file "myThermo" without any change.when I run my case,I found there are more two thermotype you defined as following:
thermoType
{
type hePsiThermo;
mixture multiComponentMixture;
transport sutherland;
thermo janaf;
energy absoluteEnthalpy;
equationOfState perfectGas;
specie specie;
}
thermoType
{
type hePsiThermo;
mixture multiComponentMixture;
transport sutherland;
thermo hConst;
energy absoluteEnthalpy;
equationOfState perfectGas;
specie specie;
}
However if I replace "multiComponentMixture" to "reactingMixture" and add "#include "reactingMixture.H" in your myThermos.C,then run command "wmake libso" and run my case,it gives me error.There have no new thermotype combination.I really do not understand.Is it related to the number in file "PaxHeaders.8962",what does other file which contain numbers use?The numbers are like:
30 mtime=1379156401.926678512
30 atime=1379156401.926678512
30 ctime=1379156401.929678475

30 mtime=1379156508.559345421
30 atime=1379156508.559345421
30 ctime=1379156508.566345333
Does the keyword "multiComponentMixture" corresponding to these numbers?If it is ,what numbers can corresponding to "reactingMixture"?please give me some advise,thank you in advance!

This sound strange! Or is it a 0-dim case, i.e. something like CHEMKIN or chemFoam?

Well, if you don't use the chemistry solver, then just get rid of this stuff altogether and use psiReactionThermo without the chemistry part.
The code in createFields.H should then look something like this (similar to PDRFoam):
Then you should actually be able to use 'myThermo' without changes, hence you use 'multiComponentMixture' instead of 'reactingMixture'.
IIRC, the 'reactingMixture' is a 'multiComponentMixture' plus some chemistryReader stuff.

Dear dkxls:
As you say,I use CHEMKIN in my solver.
I am sorry to do not understanding your words "get rid of this stuff ".what does the "stuff" refer to ?Is file of PaxHeaders.8962 or file in chemistry class?
I changed codes in my createFields.H as you say ,but do not get rid of "this stuff".My thermopysicalProperties is as following:
FoamFile
{
version 2.0;
format binary;
class dictionary;
location "constant";
object thermophysicalProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
thermoType
{
type hePsiThermo;
mixture multiComponentMixtureMixture;
transport sutherland;
thermo janaf;
energy absuluteEnthalpy;
equationOfState perfectGas;
specie specie;
}
CHEMKINFile "$FOAM_CASE/chemkin/chem.inp";
CHEMKINThermoFile "$FOAM_CASE/chemkin/therm.dat";
inertSpecie N2;

/************************************************** *******************/
when I run my case ,it gives me error : keyword species is undefined in dictionary "/home/.../thermophysicalProperties".My specises is defined in chem.inp,why it still give me error?Do you mean I have to use multiComponentMixture because my solver does not use chemistry slover?If I have to use reactingMixture ,what shoud I do?For me ,you are a kinds expert in openfoam.

This looks very much like you are using the OpenFOAM chemistry solver and the CHEMKIN reader!
I have just one recommendation for you in this case: Use sensibleEnthalpy!

Thank you for all your replys !I will have a try.

So what unspeakable deeds does one have to preform to sneak a peek at your Wilke viscosity mixture code? :D I'd be very interested in seeing how you did it.

Dear dkxls:
I have used "sensibleEnthalpy" to run my case,but the temperature is not right and it is lower than before.I think it is related to "sensibleEnthalpy" I used.I should use "absoluteEnthalpy " solver the problem.
You have said to me that :
I changed makeChemistrySolvers.C and makeChemistrySolverTypes.H in a similar way like you.But it failed.please take a look on my attachment.
As you said,the 'reactingMixture' is a 'multiComponentMixture' plus some chemistryReader stuff. So ,I must modify chemisryReader class.I found the follow codes:
I think I should instantiate the 'chemistryReader' with absoluteEnthalpy in a similar way as the above codes did. If you think my idea is right ,could you give advices how to modify the codes?I have tried many times ,but failed all.[ATTACH]Attachment 25523[/ATTACH]

my attachment
 

Dear dkxls:
I send you a private message.This is my attachmentAttachment 25829.

Dear dkxls:
Thank you for your previous replies!
I think I still have to use "absoluteEnthalpy".I am new to OpenFOAM.I had a great progress by your help about my problem ,But if I would like to solve my problemcompletely, your help is necessary for me.
According to your "myThermos.C",I add the following codes into "myThermos.C":
Then I can define the new four thermotypes like the following:

However the thermotype I want to use is
thermoType
{
type hePsiThermo;
mixture reactingMixture;
transport sutherland;
thermo janaf;
energy absoluteEnthalpy;
equationOfState perfectGas;
specie specie;
},so I add the codes:
into "myThermos.C".When I run my case ,it gave me error :
I also add the file of "mymakeChemistrySolvers.C","mypsiChemistryMode ls", I still failed with the same error.I think I should also add the file of "mymakeChemistryReaders.C",but I do not know how to do it.How should I change the codes to correct the above error?Please take a look on my attachment.Thanks in advance!After reading your replies on CFD-online,I am sure you are experted in OpenFOAM and C++.
Attachment 25835

Hi Armin,
I'm trying to create a thermo model that combines hConst thermodynamics with Sutherland transport for a multiComponentMixture. I edited a couple lines in the files you provided to do this, but when I try to wmake I get the following error:
Any suggestions for a fix?

Also I'm not clear how to link a solver against a new library, do you think you could give me a quick step-by-step? Thanks.
-B

Can you upload your modified version?

The error looks rather strange as a thermo shouldn't pull in any dependencies on AMI or the like.

I posted earlier some instructions on how to include a lib in a solver (or even a case):
http://www.cfd-online.com/Forums/ope...tml#post452252
http://www.cfd-online.com/Forums/ope...tml#post451937

Sure, I just changed a couple lines from the files you uploaded to reflect the model I want to use.

I checked your code and it seems fine.
I also don't get any compilation error, it just compiles fine!

Just to make sure:
1. You need OpenFOAM version 2.2.x
2. Compiling is done like this:
3. Linking your solver against myThermo is done by editing the options file of your solver to look like this (here e.g. reactingFoam):

Thanks, I'm still getting the same error. The full message looks like this:

I have OpenFOAM 2.2.0, I can't find where it's trying to call cyclicAMILduInterfaceField.H from, and I don't know why it would be calling that in the first place.

OK, sounds a bit strange. I doubt that it has something to do with the OF version (I never used 2.2.0 though, I upgraded directly from 2.0.x to a 2.2.x git version newer than 2.2.1).

Are these files (cyclicAMILduInterfaceField.H, ...) listed in your myThermos.dep file?
In mine they are not, actually there is no *AMI*.H file at all in my myThermos.dep.

Just to make sure:
You ran 'wclean' in the 'myThermo' directory?
And there is no old 'myThermos.dep' left? (You can savely remove the *.dep files, wmake will generate new ones.)

Otherwise, I have no idea since I cannot reproduce your error.

Those files are not in my dependency file, and I always run wclean before wmake. The only *AMI* files in myThermos.dep are *AMIFvPatch* files. I was trying to trace back from the error message what line of code was calling for this *AMILdu* file, but I can't find it.

Maybe you can help me with this: why does the Make/options file need to include a link to the $LIB_SRC/finiteVolume/lnInclude folder? I can't find anything in the .C file or .H file that link to anything there. Maybe that will help me find where the erroneous call to *AMILdu* is being made.

The files you include in your lib will include themselves new dependencies and you need to tell the compiler where to find them.

Something you could try is to change the options file to match the one in the thermo library:
https://github.com/OpenFOAM/OpenFOAM...o/Make/options

Ha! That worked! I only had to include one more line in the file,
No idea why it works now and not before, but such is the nature of programming. Thanks for your help!

Hi dkxls,
Have you shared your code to calculate the mixture viscosity and conductivity to public.

"For mixture I use the formulations due to Wilke (viscosity) and Mathur (conductivity)"

If you can share the code with me, it will be very helpful. And many thanks in advance.

Zhong