Problems with time derivative

Franko · January 25, 2015, 18:28

Hello foamers!
I have two equations (assume p and T are dimensionless volScalarFields)

1) $\frac{\partial p}{\partial t} + p = 0;$

2) $\frac{\partial p T}{\partial t} + T = 0;$

I already know

and

,

The first equation is easy:

Code:

fvScalarMatrix pEqn
(   
fvm::ddt(p) + p
);
pEqn.solve();

As you know, this is equivalent to

$\frac{p_i^{n+1} - p_i^n}{\tau} + p_i^n = 0$

Now I know $p_i^{n+1}$ for all

If I write the second equation using finite differences, I will get

$\frac{p_i^{n+1}T_i^{n+1} - p_i^nT_i^n}{\tau} + T_i^n = 0$

But what is the analogue of this equation in OpenFOAM?

If I try to use

Code:

fvm::ddt(p,T) + T

I will get the wrong equation:

$\frac{p_i^{n+1}T_i^{n+1} - p_i^{n+1}T_i^n}{\tau} + T_i^n = 0$

So how to use OpenFOAM correctly here?
Please help!

alexeym · January 26, 2015, 02:39

Hi,

If I am not mistaken

$\frac{\partial{pT}}{\partial{t}} = p\frac{\partial{T}}{\partial{t}} + T\frac{\partial{p}}{\partial{t}}$

and then using first equation:

$\frac{\partial{pT}}{\partial{t}} = p\frac{\partial{T}}{\partial{t}} - pT$

and

$p\frac{\partial{T}}{\partial{t}}$

is

Code:

fvm::ddt(p, T)

demichie · January 26, 2015, 03:18

Hi,
are you sure that about this?

Quote:

Originally Posted by alexeym

$p\frac{\partial{T}}{\partial{t}}$

is

Code:

fvm::ddt(p, T)

I've always tought that ddt(p,T) discretizes the derivative in time of pT. Otherwise, if it was p times the temporal derivative of T, why not using p*ddt(t)?
Also looking at Table 2.2 of the programming guide it seems that ddt(p,T) should be the discretization of the time derivative of (p*T).

Can you clarify it?

Thank you
Mattia

ahmmedshakil · January 26, 2015, 03:55

Quote:

Originally Posted by demichie

Hi,
are you sure that about this?

I've always tought that ddt(p,T) discretizes the derivative in time of pT. Otherwise, if it was p times the temporal derivative of T, why not using p*ddt(t)?
Also looking at Table 2.2 of the programming guide it seems that ddt(p,T) should be the discretization of the time derivative of (p*T).

Can you clarify it?

Thank you
Mattia

Yes, I think Mattia de\' Michieli Vitturi is right. To the best knowledge, it's discretised as time derivative of (p*T). To be confirmed, I guess, you can check the book "An Introduction to Computational Fluid Dynamics: The Finite Volume Method"-by H.K. Versteeg and W. Malalasekera.

Cheers
shakil

Franko · January 26, 2015, 04:13

So what is the correct formula:
1) $fvm::ddt(p,T)=\frac{p_i^{n+1}T_i^{n+1} - p_i^nT_i^n}{\tau}$

or 2) $fvm::ddt(p,T)=\frac{p_i^{n+1}T_i^{n+1} - p_i^{n+1}T_i^n}{\tau}$ ?

If you think that the first formula is right, are you sure that OpenFOAM "remember" the old p (

)?

alexeym · January 26, 2015, 04:18

Well,

Here fvc::ddt method in EulerDdtScheme:

Code:

template<class Type>
tmp<GeometricField<Type, fvPatchField, volMesh> >
EulerDdtScheme<Type>::fvcDdt
(
    const dimensionedScalar& rho,
    const GeometricField<Type, fvPatchField, volMesh>& vf
)
{
    dimensionedScalar rDeltaT = 1.0/mesh().time().deltaT();

    IOobject ddtIOobject
    (
        "ddt("+rho.name()+','+vf.name()+')',
        mesh().time().timeName(),
        mesh()
    );
    if (mesh().moving())
    {
        ...
    }
    else
    {
        return tmp<GeometricField<Type, fvPatchField, volMesh> >
        (
            new GeometricField<Type, fvPatchField, volMesh>
            (
                ddtIOobject,
                rDeltaT*rho*(vf - vf.oldTime())
            )
        );
    }
}

While fvm::ddt

Code:

template<class Type>
tmp<fvMatrix<Type> >
EulerDdtScheme<Type>::fvmDdt
(
    const volScalarField& rho,
    const GeometricField<Type, fvPatchField, volMesh>& vf
)
{
    ...
    scalar rDeltaT = 1.0/mesh().time().deltaTValue();

    fvm.diag() = rDeltaT*rho.internalField()*mesh().Vsc();
    if (mesh().moving())
    {
        ...
    }
    else
    {
        fvm.source() = rDeltaT
            *rho.oldTime().internalField()
            *vf.oldTime().internalField()*mesh().Vsc();
    }
    ...
}

demichie · January 26, 2015, 04:18

The correct formula is the first one. Take a look at the programmers guide (page 37 for version 2.3.1) and you will find everything. Eq. 2.21 is exactly what you are looking for.

Mattia

Franko · January 27, 2015, 18:35

I am not sure that I understand

correctly...

I think that in the beginning of the time loop (p and T are dimensionless volScalarFields) we have formula below:

$fvc::ddt(p,T) = \frac{p_i^n*(T_i^{n+1} - T_i^n)}{\tau}$

But after solving this equation:

Code:

fvScalarMatrix pEqn
(  
fvm::ddt(p) + p
);
pEqn.solve();

$fvc::ddt(p,T) = \frac{p_i^{n+1}*(T_i^{n+1} - T_i^n)}{\tau}$

So $fvc::ddt(rho, phi) = \frac{rho*(phi^{n+1} - phi^n)}{\tau}$ ?
I mean when we use

, rho always behaves like a scalar, right?
Please correct me, if I am wrong.

alexeym · January 28, 2015, 03:26

It behaves like scalar field i.e. it can vary in space.

Franko · January 28, 2015, 04:10

alexeym, yes, sure.

And if we have only one argument (volScalarField phi) we will get $fvc::ddt(phi) = \frac{phi^{n+1} - phi^n}{\tau}$

Now it is clear.

Franko · January 28, 2015, 16:44

Hi, I have a new big problem with temporal derivative!

Again, A and B are dimensionless volScalarFields
I also have

Code:

dimensionedScalar c ("c", dimensionSet(0, 0, 1, 0, 0, 0 ,0), 1.0);

In the beginning, I know

and

,

I solved the first equation:

Code:

fvScalarMatrix AEqn
        (
        c*fvm::ddt(A) + A
        );
AEqn.solve();

As you know, this is equivalent to

$\frac{A_i^{n+1} - A_i^n}{\tau} + A_i^n = 0$

Now I know $A_i^{n+1}, A_i^n$ and

,

After that I tried to solve the second equation:

Code:

fvScalarMatrix BEqn
        (
            c*fvm::ddt(A) +c*fvm::ddt(B) + B
        );
BEqn.solve();

It compiles, but then

Code:

--> FOAM FATAL ERROR : incompatible fields
for operation [A] + [B]

It seems that OpenFOAM don't understand that I have already calculated field $A_i^{n+1}$ in the first equation!
How can I tell him that?

Thank you very much for any hint ...

alexeym · January 29, 2015, 01:45

Hi,

fvm:: methods usually operate on the same field, so OpenFOAM is not quite happy about your fvm::ddt(A) + fvm::ddt(B). If you need time derivative of A in equation for B, you can use it as a source term with fvc::ddt(A). So your code should be:

Code:

fvm::ddt(B) + B/c + fvc::ddt(A)

(if c is scalar != 0, why not divide equations by c?)

Franko · January 29, 2015, 02:53

alexeym, exactly, I need to use fvc::ddt(A) in my equation...
Thanks a lot!

January 25, 2015, 18:28	Problems with time derivative	#1
Franko New Member Join Date: Sep 2014 Posts: 15 Rep Power: 11	Hello foamers! I have two equations (assume p and T are dimensionless volScalarFields) 1) $\frac{\partial p}{\partial t} + p = 0;$ 2) $\frac{\partial p T}{\partial t} + T = 0;$ I already know and , The first equation is easy: Code: fvScalarMatrix pEqn ( fvm::ddt(p) + p ); pEqn.solve(); As you know, this is equivalent to $\frac{p_i^{n+1} - p_i^n}{\tau} + p_i^n = 0$ Now I know $p_i^{n+1}$ for all If I write the second equation using finite differences, I will get $\frac{p_i^{n+1}T_i^{n+1} - p_i^nT_i^n}{\tau} + T_i^n = 0$ But what is the analogue of this equation in OpenFOAM? If I try to use Code: fvm::ddt(p,T) + T I will get the wrong equation: $\frac{p_i^{n+1}T_i^{n+1} - p_i^{n+1}T_i^n}{\tau} + T_i^n = 0$ So how to use OpenFOAM correctly here? Please help!

January 26, 2015, 02:39		#2
alexeym Senior Member Alexey Matveichev Join Date: Aug 2011 Location: Nancy, France Posts: 1,930 Rep Power: 38	Hi, If I am not mistaken $\frac{\partial{pT}}{\partial{t}} = p\frac{\partial{T}}{\partial{t}} + T\frac{\partial{p}}{\partial{t}}$ and then using first equation: $\frac{\partial{pT}}{\partial{t}} = p\frac{\partial{T}}{\partial{t}} - pT$ and $p\frac{\partial{T}}{\partial{t}}$ is Code: fvm::ddt(p, T)

January 26, 2015, 04:13		#5
Franko New Member Join Date: Sep 2014 Posts: 15 Rep Power: 11	So what is the correct formula: 1) $fvm::ddt(p,T)=\frac{p_i^{n+1}T_i^{n+1} - p_i^nT_i^n}{\tau}$ or 2) $fvm::ddt(p,T)=\frac{p_i^{n+1}T_i^{n+1} - p_i^{n+1}T_i^n}{\tau}$ ? If you think that the first formula is right, are you sure that OpenFOAM "remember" the old p ()?

January 26, 2015, 04:18		#7
demichie Member Mattia de\' Michieli Vitturi Join Date: Mar 2009 Posts: 50 Rep Power: 17	The correct formula is the first one. Take a look at the programmers guide (page 37 for version 2.3.1) and you will find everything. Eq. 2.21 is exactly what you are looking for. Mattia Franko likes this.

January 27, 2015, 18:35		#8
Franko New Member Join Date: Sep 2014 Posts: 15 Rep Power: 11	I am not sure that I understand correctly... I think that in the beginning of the time loop (p and T are dimensionless volScalarFields) we have formula below: $fvc::ddt(p,T) = \frac{p_i^n(T_i^{n+1} - T_i^n)}{\tau}$ But after solving this equation: Code: fvScalarMatrix pEqn ( fvm::ddt(p) + p ); pEqn.solve(); $fvc::ddt(p,T) = \frac{p_i^{n+1}(T_i^{n+1} - T_i^n)}{\tau}$ So $fvc::ddt(rho, phi) = \frac{rho*(phi^{n+1} - phi^n)}{\tau}$ ? I mean when we use , rho always behaves like a scalar, right? Please correct me, if I am wrong.

January 28, 2015, 03:26		#9
alexeym Senior Member Alexey Matveichev Join Date: Aug 2011 Location: Nancy, France Posts: 1,930 Rep Power: 38	It behaves like scalar field i.e. it can vary in space. Franko likes this.

January 28, 2015, 04:10		#10
Franko New Member Join Date: Sep 2014 Posts: 15 Rep Power: 11	alexeym, yes, sure. And if we have only one argument (volScalarField phi) we will get $fvc::ddt(phi) = \frac{phi^{n+1} - phi^n}{\tau}$ Now it is clear.

January 28, 2015, 16:44	new problem	#11
Franko New Member Join Date: Sep 2014 Posts: 15 Rep Power: 11	Hi, I have a new big problem with temporal derivative! Again, A and B are dimensionless volScalarFields I also have Code: dimensionedScalar c ("c", dimensionSet(0, 0, 1, 0, 0, 0 ,0), 1.0); In the beginning, I know and , I solved the first equation: Code: fvScalarMatrix AEqn ( cfvm::ddt(A) + A ); AEqn.solve(); As you know, this is equivalent to $\frac{A_i^{n+1} - A_i^n}{\tau} + A_i^n = 0$ Now I know $A_i^{n+1}, A_i^n$ and , After that I tried to solve the second equation: Code: fvScalarMatrix BEqn ( cfvm::ddt(A) +c*fvm::ddt(B) + B ); BEqn.solve(); It compiles, but then Code: --> FOAM FATAL ERROR : incompatible fields for operation [A] + [B] It seems that OpenFOAM don't understand that I have already calculated field $A_i^{n+1}$ in the first equation! How can I tell him that? Thank you very much for any hint ... Annier likes this.

January 29, 2015, 01:45		#12
alexeym Senior Member Alexey Matveichev Join Date: Aug 2011 Location: Nancy, France Posts: 1,930 Rep Power: 38	Hi, fvm:: methods usually operate on the same field, so OpenFOAM is not quite happy about your fvm::ddt(A) + fvm::ddt(B). If you need time derivative of A in equation for B, you can use it as a source term with fvc::ddt(A). So your code should be: Code: fvm::ddt(B) + B/c + fvc::ddt(A) (if c is scalar != 0, why not divide equations by c?) Annier and Franko like this.

January 29, 2015, 02:53		#13
Franko New Member Join Date: Sep 2014 Posts: 15 Rep Power: 11	alexeym, exactly, I need to use fvc::ddt(A) in my equation... Thanks a lot!

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Elastic or Plastic Deformations in OpenFOAM	NickolasPl	OpenFOAM Pre-Processing	36	September 23, 2023 08:22
AMI speed performance	danny123	OpenFOAM	21	October 24, 2020 04:13
simpleFoam error - "Floating point exception"	mbcx4jc2	OpenFOAM Running, Solving & CFD	12	August 4, 2015 02:20
Moving mesh	Niklas Wikstrom (Wikstrom)	OpenFOAM Running, Solving & CFD	122	June 15, 2014 06:20
Micro Scale Pore, icoFoam	gooya_kabir	OpenFOAM Running, Solving & CFD	2	November 2, 2013 13:58