[bullmut]

Hi All

I am switching to openFOAM 4 from 2.3.1
Currently working on the postProcess utility. I have run the motorbike tutorial to get a understanding on the new syntax. I then disabled the #inlcude files in the controlDict. I did this to try and run those files through the postProcess utility. I had sucess with
"streamlines" -

postProcess -func streamLines

and
"cuttingPlane" -

postProcess -func cuttingPlane

However
"forceCoeffs" -

postProcess -func forceCoeffs

and
"wallBoundedStreamLines" -

postProcess -func wallBoundedStreamLines

wont work directly.
so this is a two part question. Can anyone explain why these files wont work through this utility? In the case of the the forceCoeffs file i get the following error:

--> FOAM FATAL ERROR: 
Could not find U, p

and for the wallBoundedStreamLines, the error that pops up revolves around it not seeing a UNear field in the time folder.

--> FOAM FATAL ERROR: 
Cannot find field UNear
Valid scalar fields are:
2
(
k
p
)

Valid vector fields are:1(U)

But within the file itself it asks OF to make the UNear field.
So i then tried to run the nearWallField section of the file alone. I have not altered the file in anyway, i cut the one dictionary out form the original wallBoundedStreamLines file, and ran the code attached and got the following error

--> FOAM FATAL IO ERROR: 
wrong token type - expected word, found on line 19 the punctuation token '('

file: /home/erfort/OpenFOAM/erfort-4.0/tutorials/incompressible/simpleFoam/motorBike/system/near.near.fields at line 19.

    From function Foam::Istream& Foam::operator>>(Foam::Istream&, Foam::word&)
    in file primitives/strings/word/wordIO.C at line 74.

FOAM exiting

Then i removed the brackets around the field specification and got this...

--> FOAM FATAL IO ERROR: 
Expected a '(' while reading Tuple2, found on line 19 the word 'U'

file: /home/erfort/OpenFOAM/erfort-4.0/tutorials/incompressible/simpleFoam/motorBike/system/near.near.fields at line 19.

    From function Foam::Istream& Foam::Istream::readBegin(const char*)
    in file db/IOstreams/IOstreams/Istream.C at line 92.

Any advice on what is going on? I have read through the documentation with no success. Am i using this utility right? If the file has more than one subdictionary (like in wallboundedStreamLines) should i change the command line? How come forcesCoeff doesnt see fields that are present in the time directory?
I look forward to the replies

Regards

[igor.leo93]

Hello

Take a look here:
http://cfd.direct/openfoam/user-guid...#x31-2270006.2

For the first function, try this :

postProcess -fields "(p U)" -func forceCoeffs

About that second one i'm not sure, but i will take a look at it later.

Regards,
Igor Carvalho

[bullmut]

Hi Igor

Thanks for the reply,
I tried using the line you suggested, it now reads the fields , but got the following reply

--> FOAM FATAL ERROR: 
No valid model for viscous stress calculation
    From function Foam::tmp<Foam::GeometricField<Foam::SymmTensor<double>, Foam::fvPatchField, Foam::volMesh> > Foam::functionObjects::forces::devRhoReff() const

I noticed at the post you directed me to, was the built in fucntion file for forcecoeffs.
I then ran the following line

postProcess -func 'forcesIncompressible('bladeBot',p,U)'

And got the same error. so i think i need to add into my fvSchemes file a definition for "devRhoReff", correct?

Full output in attachment

Regards

[igor.leo93]

Hello

Well i'm not quite sure my friend.
I never had to use that function before so i can't say for sure, but i think that is correct, try that.
Let us know if it works.

Regards

[bullmut]

solution... READ THE USER GUIDE.
So while i have read the user guide more than once, they tend to update along with the openFOAM versions.
The solution to my problem was to add the solver info.

simpleFoam -postProcess -func 'forces' -latestTime

The solver then provides field information as well as turbulence model.

Had i read the book... i would see said answer.
Thanks Igor for the help though. Each step counts!

Hope this helps someone eventually

[igor.leo93]

Yeah nice.
Now that i look at the error you were getting i realize that the solver info was needed, it is good habit perhaps, to also use the solver info on all functions for postprocessing.

Best regards,
Igor

[Dan N]

Hey All

I am trying to use the postProcess utility to calculate a patch average by using:

postProcess -func 'patchAverage'

it tells me that it needs a patch name:

surfaceRegion patchAverage: patch(<patchName>):
Unknown patch name: <patchName>. Valid patch names are:
3
(
movingWall
fixedWalls
frontAndBack
)

But it seems that i cant finde a way to specify that patch name, can anyone help me?

[bullmut]

Hi Dan
After you specify the function you also need to tell it where to look.
try the following

postProcess -func "patchAverage(field,name=fixedWalls)"

The field you are interested in will be called on the patch you named

[Dan N]

Hi bullmut

Thanks it works.

Dan.

[harvee]

Hey all
I want to calculate the gradient of density and velocity.

Here is what I type:

postProcess -fields '(rho U)' -func 'grad'

Returns:

Reading fields:
volScalarFields: rho
volVectorFields: U

Executing funtionObjects
-->FOAM Warning : fuctionObject grad: Cannot find require field <fieldName>

anyone know how to fix it?
Thanks

[bullmut]

Hi Harvee

Try the line

postProcess -func "grad(U)"

It should act through the whole field and save the field to each time step.

[harvee]

Hi bullmut
thanks for the quick reply.

I tried your code get I get this:
Executing functionObjects
--> FOAM Warning :
From function bool Foam::functionObjects::regionFunctionObject::store (Foam::word&, const Foam::tmp<T>&, bool) [with ObjectType = Foam::GeometricField<Foam::Tensor<double>, Foam::fvPatchField, Foam::volMesh>]
in file home/OpenFOAM/OpenFOAM-4.0/src/OpenFOAM/lnInclude/regionFunctionObjectTemplates.C at line 61
Cannot store cache-able field with the named used in the cache.
Either choose a different name or cache the field and use the 'writeObjects' functionObject.
--> FOAM Warning : functionObject grad: Cannot find required field U

I tried a lot of combination of fields and func ,none of them worked.

and when I try to get grad(rho), the rho file doesn't exist in my 0 folder since I'm using
rhoCentralFoam, I thought that maybe affect the searching of rho, do you know how to calculate rho for 0 folder btw?

[hsalem]

Hi Dear friends,
I have problem with using post processing tool. When I want to use the Force coefficient tool to find out about Cl, Cd, Cm there is problem with this type:
--> FOAM FATAL ERROR:
Could not find rho

From function void Foam::functionObjects::forces::initialise()
in file forces/forces.C at line 197.

FOAM exiting
Any idea?
this is my Code:
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration |
\\ / A nd | Web: www.OpenFOAM.org
\\/ M anipulation |
-------------------------------------------------------------------------------
Description
Calculates lift, drag and moment coefficients by summing forces on
specified patches for a case where the solver is incompressible (pressure
is kinematic, e.g. m^2/s^2).

\*---------------------------------------------------------------------------*/
forces
{
type forces;
functionObjectLibs ("libforces.so");
writeControl timeStep;
writeInterval 10;

patches ( "airfoil.*" );
pName p;
UName U;
rhoName rhoInf;
log true;

CofR (0.25 0 0);

rhoInf 1.284;
}


forceCoeffs
{
type forceCoeffs;
functionObjectLibs ( "libforces.so" );
writeControl timeStep;
writeInterval 10;

patches ( "airfoil.*" );
pName p;
UName U;
rhoName rhoInf;
log true;

liftDir (0 1 0);
dragDir (1 0 0);
CofR (0.25 0 0);
pitchAxis (0 0 1);

magUInf 6.69;
rhoInf 1.284;
lRef 1;
Aref 1;
}

[harvee]

Hey there!
grad(U) func seems can only deal one time directory once a time.
Until the bug is resolved, you can only calculate grad(U) for one time directory. You can add one of the time options, e.g -time <timeDir> or -latestTime, to select a specific time directory. For all time directories, the following will work in the meantime,make a script and put this in:

for d in $(foamListTimes) ;
do postProcess -time $d -func "grad(U)" ;
done

Additional info:

for machNo
solvername -postProcess -func MachNo

many command seems need to specify the solvername. The point about Mach number is you cannot do "pure" post-processing using data in time directories, because it also requires thermophysical models.

[harvee]

try this:
<solvername> -postProcess -func "forceCoeffsCompressible"

[hsalem]

Thank you harvee for your time.
your suggestion will work after the simulation is done. but I this problem doesn't let the simulation start. am I right? if not, where should I include your suggestion?

[harvee]

Originally Posted by hsalem

Thank you harvee for your time.
your suggestion will work after the simulation is done. but I this problem doesn't let the simulation start. am I right? if not, where should I include your suggestion?

hi hsalem
Maybe I misunderstood your problem.
you're right,my case is doing some post-process after the simulation is done.
I've never used Run-time data processing.sorry I can't help you.
the only thing I can find related is on this page:http://cfd.direct/openfoam/user-guid...#x31-2270006.2
let me know if you figure it out.

[hsalem]

Dear Harvee,
Thank you. Yes I have found the solution. it seems that I was using the old method of finding the force coefficients. in openfooam 4, there is a package that let you use it more easily. all you need is to see the user guide section 6.2.2.

[VIJAYA KUMAR]

Dolution

After lots of trouble this works

I used in pimpleFoam solver. In OF4.0 it is necessary to specify the solver name

pimpleFoam -postProcess -func "grad(U)"

[Endel]

Helly everyone,

I am trying to calculate the rho field from a sonicFoam case.

In previous versions of OpenFOAM this was apparently possible using

execFlowFunctionObjects

as described here:

https://www.cfd-online.com/Forums/op...tml#post254920

In OF4 however, this doesn't seem to work anymore and the following message appears:

execFlowFunctionObjects has been superceded by the '-postProcess' solver command-line option

I still can't figure out how to calculate the rho field by either using the postProcess utility or the former solution above.

Any help is highly appreciated, thank you very much!