|
[Sponsors] |
June 28, 2007, 09:03 |
I am trying to include a new e
|
#1 |
Member
Tomislav Sencic
Join Date: Mar 2009
Posts: 42
Rep Power: 17 |
I am trying to include a new equation in dieselEngineFoam.
I included: fvScalarMatrix sootEqn solve ( fvm::ddt(rho, soot) + fvm::div(phi, soot) == 0.5*mag(U) ); In createFields.H I defined the field by: volScalarField soot ( IOobject ( "soot", runTime.timeName(), mesh, IOobject::MUST_READ, IOobject::AUTO_WRITE ), mesh, dimensionedScalar("zero", dimensionSet(1,-3,-1,0,0,0,0), 0.0) ); It compiles, but at the beginning of the run I recive the error: --> FOAM FATAL ERROR : valueInternalCoeffs cannot be called for a calculatedFvPatchField. You are probably trying to solve for a field with a calculated boundary conditions. From function calculatedFvPatchField<type>::valueInternalCoeffs( const tmp<scalarfield>&) const in file fields/fvPatchFields/basicFvPatchFields/calculated/calculatedFvPatchField.C at line 136. FOAM exiting What does it mean? How can I solve it? Tomislav |
|
June 28, 2007, 10:18 |
What it means is: "I created a
|
#2 |
Assistant Moderator
Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,225
Rep Power: 51 |
What it means is: "I created a field with no defined boundary conditions. This is OK. But you want me to solve an equation without BCs. This is not OK"
Get rid of the last parameter for your soot field. Instead create a soot file in your 0 directory with intial-BC(==0), dimensions AND boundary conditions
__________________
Note: I don't use "Friend"-feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request |
|
June 29, 2007, 07:40 |
Thanks, it helped.
But, whe
|
#3 |
Member
Tomislav Sencic
Join Date: Mar 2009
Posts: 42
Rep Power: 17 |
Thanks, it helped.
But, when I set the soot dimensions in the 0 directory to: dimensions [0 0 0 0 0 0 0]; I obtain: --> FOAM FATAL ERROR : incompatible dimensions for operation [soot[1 -3 -1 0 0 0 0] ] == [scal[0 0 0 0 0 0 0] ] Where else could be defined the soot dimensions, where does come from the [soot[1 -3 -1 0 0 0 0] ] dimension? |
|
June 29, 2007, 08:41 |
soot is the dimension of the r
|
#4 |
Assistant Moderator
Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,225
Rep Power: 51 |
soot[1 -3 -1 0 0 0 0] is the dimension of the right hand side (density per second) - the ddt ad div seem to be consistent. What seems to be wrong is the dimension of the right hand side. You've got to add a dimensioned scalar that has the right dimension (but think about the physical meaning of that)
__________________
Note: I don't use "Friend"-feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request |
|
July 2, 2007, 11:17 |
I meant to say "left side" in
|
#5 |
Assistant Moderator
Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,225
Rep Power: 51 |
I meant to say "left side" in my last post. rho has dimension [1 -3 0 0 0 0 0] ddt adds [0 0 -1 0 0 0 0] with your undimensioned soot the resulting dimension is [1 -3 -1 0 0 0 0]
How many iterations does the linear solver need to get to "internalField uniform 0;"? What are the boundary conditions for soot? Try without a source term, but with an inhomogenous initial distribution of soot.
__________________
Note: I don't use "Friend"-feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request |
|
July 3, 2007, 07:07 |
OK, I got the dimensions.
I
|
#6 |
Member
Tomislav Sencic
Join Date: Mar 2009
Posts: 42
Rep Power: 17 |
OK, I got the dimensions.
I do not know the number of iterations because in the log file "soot" is never mentioned, there is no something like: BICCG: Solving for soot, Initial residual = 1, Final residual = 1.53774e-08, No Iterations 5 Could this be the key of the problem? I tried the other things you suggested, but without result. The boundary conditions are: boundaryField { piston { type zeroGradient; } liner { type zeroGradient; } cylinderHead { type zeroGradient; } cyclic { type cyclic; value uniform 0; } |
|
July 3, 2007, 07:10 |
ON, so you've got a field with
|
#7 |
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,905
Rep Power: 33 |
ON, so you've got a field with zero gradient or cyclic b.c.-s all the way around and I suspect a uniform internal field. Do you have any sources or sinks in the equation or does the current solution satisfy the equations already?
If it does, OpenFOAM won't bother solving for it. Hrv
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
User defined bc | anja | OpenFOAM Running, Solving & CFD | 20 | June 6, 2008 12:12 |
User-Defined Fan | Socrate | FLUENT | 0 | March 28, 2007 10:25 |
User Defined GUI | Frederik | FLUENT | 0 | June 23, 2006 16:12 |
user defined scalars | ramesh | FLUENT | 1 | June 11, 2004 17:25 |
user defined viscosity | solomon | FLUENT | 0 | July 13, 2003 21:09 |