doubt with fluent
I am working in a steady state problem using fluent. If i am using a turbulent solver from the beginning, it gives physically unrealistic results. However if i use the laminar solver first and then after some iterations switch to turbulent model, results are physically meaningful. Is there anything wrong in this procedure?..of first using the laminar solver and then using the solution as initial solution to the turbulent flow.. Any help will be highly useful.

Re: doubt with fluent
Keep in mind that when one is solving for the turbulent case instead of the laminar case, more equations are required to be solved per each numerical iteration. That is why your laminar solution seems to be more accurate for the first set of iterations. When a solution is given an improved set of intial conditions, the solution should converge quicker and may obtain increased accuracy. It is advisable to obtain simpler solutions for a starting point and then change your models and solution controls for an improved solution. It may be best to begin with an inviscid model, and allow for minimal convergence (perhaps convergence criterion = 0.001). This will get you in the ballpark. Then change your model to laminar, and allow for convergence to a similar minimal convergence (0.001 or maybe 0.0001). From this point you can patch in this solution as your initial conditions for a solution with a turbulence model. At this time you can also enable the energy equation, change discreitization schemes, change the steady state solution to an unsteady case if desired, etc. You should also increase your convergence criterion up to the range of 1e6 to 1e9. Does this help?

Re: doubt with fluent
Thanks chetan...

Re: doubt with fluent
(1). The flow field of a laminar flow is very different from that of the turbulent flow. So, there is no advantage of solving the laminar flow first. (2). And even if you have the laminar flow solution, you still don't have the turbulence quantities such as the turbulence kinetic energy, the tke dissipation, the eddy viscosity. These quantities are not consistent with the laminar flow field. (3). I have never used this approach before, and I think, if you control the relaxation factors gradually, you can achieve the solution convergence by solving the turbulent flow equations right from the begining. (4). In using one of the commercial cfd code, the initial flow field can be obtained easily through interpolation of the coarse mesh solution, which normally is easier to converge (than the fine mesh solution.) (5). I think, it is a much better apporach to run a coarse mesh solution first. In this way, most of the flow variables will be self consistent. (6). The other way to do is to activate the multigrid options. This will also speed up the convergence of a fine mesh solution. (7). I still think, I need to remind you of the mesh independent solution issue. So, even if the solution looks reasonable, you still have to push harder to obtain a mesh independence solution through a systematic mesh refinement. (8). So, based on my experience of using commercial codes (including the one you mentioned), there was no need to first solve the laminar flow problem, even for very complex 3D problems.

All times are GMT 4. The time now is 03:50. 