code_saturne User's Forum

Hi all,
 
Here I am again, facing difficulties to obtain a converged solution for a case I am studying. I am trying to simulate an internal flow in an autoclave, with an object placed in it. My geometry is symmetrical, so I modeled only a half of it. Basically it is a half cylinder with a big complex object in it. The air is blown in the autoclave through an opening all around the cylinder and there is a turbine on the opposite wall which sucks the air. My boundary conditions are : imposed velocity at the inlet and the outlet (the velocity at the outlet is calculated so that the air flow at the inlet is the same as the one at the outlet), other boundaries are smooth non sliding walls. My mesh is fine enough, and the cells meet quite good quality criteria.
 
First, I wanted to have a converged solution for a laminar flow (even is the flow is fully turbulent, it was just to see how Code Saturne would deal with this quite complex case)... it seems that I am unable to do so. I tried changing some parameters, as the convergence criteria (1e-3 -> 1e-5) and relaxation factor (0.6 for u,v,w and 0.1 for p). My questions are : 
 
1) is it possible that modeling a fully turbulent flow without any turbulence model could be problematic to have a converged solution (I don't want here a perfectly realistic solution, just something that converges so then I can deal with turbulence knowing that everything else works fine) ? 
2) at the beginning and at the end of the calculation, I have a warning : mesh not enough refined at the wall for to run laminar calculation. Can this be the source of the divergence ?
3) I use the IMRGRA=3 for the gradient calculation method (least squares method over partial extended cell neighborhood). Is it the best choice ?
4) which other parameters can lead to a divergence of the calculation ? (I mean numerical parameters, not related to the geometry or mesh) I use the centered scheme to discretise u, v and w.
5) which turbulence model do you think is the most appropriate (knowing that the goal of my study is to model heat transfer (convection, conduction, radiation, coupling with syrthes) in the autoclave)
 
I attach here the xml file of the laminar calculation, but I can not attach the listing as the last one I got is 3go big (I can not even open it myself... a lot of iterations (500) and divergence at the beginning (it 50 approximatively), with an error message printed at each iteration and for each wall face : max nb of iterations reached for the calculation of uet NTIM=100, desired precision EPS=0,1e-2, CAUSTA subroutine called for face IFAC=xxx). The only thing I know for this calculation is that for at least one iteration, the maximum number of iteration for the pressure calculation (conjugate gadient) has reached the max 10000, and so the precision 1e-5 is not reached. I should have another listing file in the afternoon as I have the same calculation running right now for only a few iterations.
 
Thanks all in advance for you help,

Alicia

Hello,

Here are a few answers:

1) Modeling a turbulent flow with no turbulence model may be impossible if the Reynolds numbers are too high and the flow should be unstable. If you want to test your mesh with no turbulence model, you may do so by increasing the fluid's viscosity so that the flui really is laminar (do not forget to reset the true viscosity when you switch your turbulence back on).
2) the warning : "mesh not enough refined at the wall for to run laminar calculation" might be the source of the divergence, but this seems quite improbable (except as for how it relates to 1)
3) IMRGRA 2 or 3 are what we usually recommend. The gradients computed with these options might not always be more precse than with IMRGRA = 1 (judging by usual "code_saturne check_mesh" results), but they are usually smoother. So IMRGRA=3 is expected to be the best choice, though testing other options may be interesting.
4) The first thing I would try would be to use a standard "free outlet" condition at the outlet. Your velocity profile may not be exactly the same as at the inlet, but total outflow will still be equal to total inflow, and you reduce the risk of trying to impose slightly different inflows and outflows due to a slightly different curved surface area (some collegues use this type of forced outlet = inlet boundary condition regularly with no issues, but if you have curved inflow and outflow surfaces, you must be very cautious to calculate to total "discrete" inflow, the total "discrete" outflow, and assign a multiplicative factor to the outflow if the totals do not quite match.

Otherwise, for tetrahedral or curved/streched hexahedral meshes, it is always a good bet to try using "relaxation of pressure increase" in case of divergence (a relaxation factor of .8 or even .9 is usualy enough).
If those still fail, using a an 80%centered/20% upwind scheme instead of 100%centered may help.

5) As to the most appropriate turbulence model, this is a tricky question, which will depend on whether the flow is high or low-Reynolds near the wall, and possibly on other flow characteristics. The k-omega SST model is reputedly good for dynamics but bat at thermal exchange prediction, so I would not recommended it. As for the others, you may find more comparison data on the University of Manchester's "Twiki" here : http://cfd.mace.manchester.ac.uk/twiki/bin/view/Saturne/TestCases

Best regards,

  Yvan