[mrangitschdowcom]

Hi all,
I'm having fits with a non-reacting case mixing fluids with different temperatures. I'm continually getting a temperature out of range error in the janafThermo routines. The domain is a quarter of a pipe, with zero gradient boundaries on the walls, and quarter symmetry used (2 symmetry planes). Looking at the data, the boundary value at the input has the correct value (300K). The temperatures at the wall of the inlet plane and the symmetry edges of the inlet plane go down as the solution progresses, eventually giving me the low temperature error.
I've tried restricting the courant number to 0.1 (and lower), but it just delays the problem. I'm using OpenFoam 1.3 on a linux box...

Any hints would be appreciated...

Mike

[hjasak]

Sounds like a boundry condition problem to me... Let's investigate:

First, check the mesh: is the non-orthogonality bad. Running checkMesh should tell you all you need to know.

Second, check if you are satisfying continuity. Have a look at local and global continuity error: they should be of the same order of magnitude as the pressure solver convergence tolerance. If this is too big, try tightening the pressure tolerance.

If all is well, let's try first order discretisation: switch the convection discretisation to upwind and diffusion to Gauss linear limited 0.5. If the error does not go away, I'm pretty sure it's your boundary conditions.

Keep us posted,

Hrv

[mrangitschdowcom]

Hi Hrvoje,
The grid checked out just fine. OK's on all parameters (it's a mixed grid, but the part with problems was nice, uniform hex's, very orthogonal).
I tightened down on the pressure convergence tolerance (10e-12 instead of 10e-9), as you suggested. It seems to be working. The walls and and symmetry boundaries at the inlet are picking up the correct (inlet) temperature, and there are no excursions below the inlet value anywhere in the domain.
Thanks for the help!

Mike

[hjasak]

Hi Mike,

The tolerance sounds awfully tight (might be necessary though). Is this by any chance a very large hex+tet grid with lots of flow in the hex part and nothing much happening in a big tet box?

You bay be better off trying the AMG solver on the pressure equation - that has got better smoothing properties and may let you get away without such tight convergence. In any case, it should be faster...

Hrv

[mrangitschdowcom]

Hi again Hrvoje,
The domain is two cocentric cylinders connected by a couple holes (the inner cylinder is capped off). The tet grids are near the holes, where the two hex grids meet. Where the flow goes through the hole, the grid is actually triangular wedges. I've imported the grid from Gambit.
I'm trying to initialize the flow to simulate an ignition. I'll try switching to the AMG solver for pressure and see what happens.

Thanks again for the help...

Mike

[mrangitschdowcom]

Hello again all,
I've been doing other things, but the problem didn't go away, it just took longer to become evident. The temperature at the symmetry planes continually decreases until I get the janaf bound error. The flow field looks correct, but

[ulrich]

Hello,

I had a maybe similar problem with reactingFoam. I did not define for all reactants the conditions at startTime. I thought this is done with the definition of ydefault. The simulations later showed that the symmetryplane was treated like a wall regarding this one reactant. The problem disappeared with explicitly defining the conditions for this reactant at startTime.

Ulrich