CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Gradient operator implicit discretization

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree1Likes
  • 1 Post By hjasak

Reply
 
LinkBack Thread Tools Display Modes
Old   November 29, 2006, 05:54
Default In order to build a solver for
  #1
New Member
 
diego n.
Join Date: Mar 2009
Posts: 17
Rep Power: 7
diegon is on a distinguished road
In order to build a solver for combustion I need to discretize the radiative transfer equation.
The RTE contains the term:

s*grad(I)

where I is a scalar and s a vector.
My problem comes from the gradient operator for which is avaible only the explicit representation but I need an implicit form to solve for I.
So I have thought to use some math and rewrite it in a form containg operator having an implicit discretization such as divergence:

s*grad(I)=div(s*I)-I*div(s)

Should it work?
diegon is offline   Reply With Quote

Old   November 29, 2006, 07:32
Default Yep, looks correct, should wor
  #2
Senior Member
 
Markus Hartinger
Join Date: Mar 2009
Posts: 102
Rep Power: 7
hartinger is on a distinguished road
Yep, looks correct, should work.

surfaceScalarField sf = fvc::surfaceInterpolate(s)& mesh.Sf();
& mesh.Sf()
s * grad(I) := fvm::div(sf, I) - fvm::Sp(fvc::div(fs), I);

the 'Sp' - thing adds a coefficient to the diagonal of the implicit matrix.

Taking this opportunity, why is there no implicit grad implementation? Anybody?

pierre and markus
hartinger is offline   Reply With Quote

Old   November 29, 2006, 07:34
Default ignore second & mesh.Sf()
  #3
Senior Member
 
Markus Hartinger
Join Date: Mar 2009
Posts: 102
Rep Power: 7
hartinger is on a distinguished road
ignore second & mesh.Sf()

P & M
hartinger is offline   Reply With Quote

Old   November 29, 2006, 07:50
Default Implicit gradient operator:
  #4
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,729
Rep Power: 20
hjasak will become famous soon enough
Implicit gradient operator:

- firstly, the diagonal would be zero.
- secondly, the matrix coefficients would be vectors for a gradient and vectors transpose for a divergence
- thirdly, you cannot solve the equation

grad(thingy) = rhs

beucase the diagonal of the gradient matrix equals zero for a uniform mesh

Implicit gradient matrix makes sense only for implicit block coupled (e.g. pressure velocity) algorithms, and I'm pretty sure noone is quite there yet with OpenFOAM.

Hrv
chegdan likes this.
__________________
Hrvoje Jasak
hjasak is offline   Reply With Quote

Old   November 29, 2006, 08:54
Default The equation I need to discret
  #5
New Member
 
diego n.
Join Date: Mar 2009
Posts: 17
Rep Power: 7
diegon is on a distinguished road
The equation I need to discretize is not

s*grad(I)=div(s*I)-I*div(s)

but it contains the "s*grad(I)" that I have thought to sobstitute it with "div(s*I)-I*div(s)".
diegon is offline   Reply With Quote

Old   November 29, 2006, 09:24
Default Hrv, thanks, does make sense.
  #6
Senior Member
 
Markus Hartinger
Join Date: Mar 2009
Posts: 102
Rep Power: 7
hartinger is on a distinguished road
Hrv, thanks, does make sense.

Diego, we decribed the implementation of "s*grad(I)" as "div(s*I)-I*div(s)", which would be one of the terms for the matrix setup (:= means defined as)

fvScalarMatrix yourEqn
(
...
+ fvm::div(sf, I) - fvm::Sp(fvc::div(fs), I)
...
);

PM
hartinger is offline   Reply With Quote

Old   November 29, 2006, 09:35
Default Ok thanks so it seems it c
  #7
New Member
 
diego n.
Join Date: Mar 2009
Posts: 17
Rep Power: 7
diegon is on a distinguished road
Ok thanks

so it seems it could not work.
diegon is offline   Reply With Quote

Old   November 29, 2006, 09:48
Default yes, it can you can't have
  #8
Senior Member
 
Markus Hartinger
Join Date: Mar 2009
Posts: 102
Rep Power: 7
hartinger is on a distinguished road
yes, it can

you can't have the term "s*grad(I)" implicitly, but you can replace that with the term you suggested "div(s*I)-I*div(s)", for which we gave the actual implementation.
The "fvm::"-prefix means in Foam-speak implicit. More precise, it is the "fvm" namespace in which all implicit functions for the Finite Volume Method (fvm) are defined.

"fvc::" denotes "Finite Volume Calculus", all explicit stuff.

So again, your reasoning is right, you can do it as you suggested.

P & M
hartinger is offline   Reply With Quote

Old   November 29, 2006, 09:55
Default Sorry but I did not get what J
  #9
New Member
 
diego n.
Join Date: Mar 2009
Posts: 17
Rep Power: 7
diegon is on a distinguished road
Sorry but I did not get what Jasak was writing so I guessed it would not have worked.

Thank you again.
diegon is offline   Reply With Quote

Old   December 27, 2006, 06:23
Default Hi Diego, I think that "s"
  #10
New Member
 
matteo cerutti
Join Date: Mar 2009
Location: Florence, Tuscany, Italy
Posts: 10
Rep Power: 7
matteoc is on a distinguished road
Hi Diego,

I think that "s" is a const vector, once u have decided the direction of the radiation...
so div(s) must be equal to zero.

So, I think u can write:
s&grad(I) = div(sI)

bye
M
matteoc is offline   Reply With Quote

Old   May 2, 2007, 05:52
Default Hi This might be a dumb que
  #11
Member
 
Erik Arlemark
Join Date: Mar 2009
Location: Eindhoven, Netherlands
Posts: 47
Rep Power: 7
Erik is on a distinguished road
Hi

This might be a dumb question but is this why the pressure is solved in a semi-discretised form of the momentum equation (A and H decompositions and solving through Jacobi metod) i.e. to find another way of implementing an implicit form of grad(p)?

/Erik
Erik is offline   Reply With Quote

Old   May 2, 2007, 05:58
Default Do you know CFX? They impleme
  #12
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,729
Rep Power: 20
hjasak will become famous soon enough
Do you know CFX? They implement a pressure-based block solver and they indeed have an implicit grad (and div!) to form a 2x2 block matrix system.

No such thing in OpenFOAM at the moment.

Hrv
__________________
Hrvoje Jasak
hjasak is offline   Reply With Quote

Old   May 2, 2007, 06:22
Default Thank you Hrv! I guess this
  #13
Member
 
Erik Arlemark
Join Date: Mar 2009
Location: Eindhoven, Netherlands
Posts: 47
Rep Power: 7
Erik is on a distinguished road
Thank you Hrv!

I guess this is the reason for the special treatment of grad(p) then.

I dont know about CFX. I am fairly new to the field of CFD and keen on using and learning more about OpenFOAM.

My problem is that I am trying to implement a different momentum equation involving gradients of density as well as the gradient of pressure. I would like to know how to formulate this in a similar manner to the one done in the PISO-loop. Ive looked through your Ph.D and found some information on the subject but I would like to see some DOC (if available) on how to get the momentum equation in the semi-discretised form. Is such DOC available to your knowledge?

regards
/Erik
Erik is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
FvPatchScalarField access operator maka OpenFOAM 3 July 1, 2008 08:32
Implicit Formulation of Velocity Gradient stefan82 OpenFOAM Running, Solving & CFD 1 August 9, 2007 11:09
Operator Splitting. Maria. Main CFD Forum 5 September 17, 2005 22:10
Operator precedence hemph OpenFOAM 1 September 13, 2005 12:40
a math operator in UDF lichun Dong FLUENT 7 June 18, 2005 22:04


All times are GMT -4. The time now is 03:27.