Turbulent viscosity

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

 November 3, 2000, 00:43 Turbulent viscosity #1 rafat Guest   Posts: n/a Dear all, I am trying to simulate a flow over a building in 2D. although the solution converged, I still recieve a message says that the turbulent viscosity ratio over the limit 1e5. I will be glad to hear any suggestions best regards, rafat

 November 3, 2000, 01:25 Re: Turbulent viscosity #2 John C. Chien Guest   Posts: n/a (1). You need to find out whether the solution you obtained is good, accurate, or mesh independent. (2). How do you simulate flow over a building in 2-D? I have never heard of a 2-D building. (3). Anyway, you need to pay attention to the mesh, and the Y+ constraint next to the wall. (Assuming that you are using the standard k-epsilon turbulence model, then the Y+ next to the wall must be in the universal log-law profile region.)

 November 6, 2000, 18:54 Re: Turbulent viscosity #3 Sung-Eun Kim Guest   Posts: n/a I suggest you plot (contour) the turbulent viscosity ratio in the domain and see where it exceeds 10**5. In fact, the value of 10**5 doesn't have much meaning (After all, turbulent viscosity is an artifact). We could've set it to 10**6. It's just a reminder that somewhere, in the domain, turbulent viscosity is very high. Chance is that the solutions are not fully converged, even though the residuals seem low enough. Try tighter convergence criteria. It may be due to unrealistically high turbulence intensity you're using at the inlet boundary.

 November 7, 2000, 06:04 Re: Turbulent viscosity #4 Volker Pawlik Guest   Posts: n/a Hi, lately I got the same message (for a not negligible amount of cells) in a flow with mixed convection (forced and free). In my case it helped to change the discretization scheme for pressure from 'body force weighted (bfw)' to '2nd Order', to perform some hundred iterations and then to switch again to bfw. In another case I tried to get rid of that mesaage by refining the grid where high values of the viscosity ratio occured. Unfortunately it did not help in this situation. Maybe decreasing the viscosity relaxation factor could help the prevent the solver from "creating" to much turbulence respectively turbulent viscosity.

 November 8, 2000, 00:11 Re: Turbulent viscosity #5 rafat Guest   Posts: n/a > Dear Sung-Eun Kim, : Thank you for your great advice. Actually, I set k-e equal to 1 at the : inlet which I presume it is a littel bit high. : Again I appreciate your recommendations and I will take for sure as aguid : lines to my work in the future. : : Best regards, : : Ra'fat Al-Waked : :

 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 cfdiscool FLUENT 10 June 10, 2015 06:15 Felipeb Main CFD Forum 1 July 26, 2010 17:02 shib FLUENT 0 June 22, 2010 12:44 nuimlabib Main CFD Forum 0 August 4, 2009 00:05 David Yang FLUENT 3 June 3, 2002 06:13

All times are GMT -4. The time now is 19:46.

 Contact Us - CFD Online - Top