# doubt with fluent

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 October 30, 2000, 05:55 doubt with fluent #1 G.Balakrishnan Guest   Posts: n/a 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.

 October 30, 2000, 06:21 Re: doubt with fluent #2 Chetan Kadakia Guest   Posts: n/a 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 1e-6 to 1e-9. Does this help?

 October 30, 2000, 06:58 Re: doubt with fluent #3 G.Balakrishnan Guest   Posts: n/a Thanks chetan...

 October 30, 2000, 22:40 Re: doubt with fluent #4 John C. Chien Guest   Posts: n/a (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 multi-grid 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 3-D problems.

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post s.mishra FLUENT 1 April 5, 2016 06:47 iņigo FLUENT 3 February 28, 2011 14:04 syadgar FLUENT 1 September 8, 2009 16:41 lzgwhy FLUENT 0 August 26, 2009 06:41 David FLUENT 11 November 14, 2000 15:32

All times are GMT -4. The time now is 00:30.

 Contact Us - CFD Online - Privacy Statement - Top