# Flow in pipes

 Register Blogs Members List Search Today's Posts Mark Forums Read

 December 30, 2001, 14:43 Flow in pipes #1 Samuel Calabrés Guest   Posts: n/a I am trying to carry out a solution for flow in a standard pipe. Due to several incovenients, I must use a code usually used for naval cases. I'm wondering if this code is usefull for me, becouse the results I get are not realistic. Should I obtain another code? The boundary conditions I am imposing are the following: celerity at the inlet flow cross section given; a roughness wall law (unused commercial steel, k=0.05E-6 m); Smagorinsky formulation of turbulence (the flow I'm considering is always turbullent, Re>10E5). Is that correct? I think the mesh is OK, so the problem is not in that way. This is a first simulation to obtain the loss of pressure/velocity because of the roughness, then I want to get the velocity and pressure fields over a valve situated in the pipe. This is where I began, but the results were not correct, so I thought I could estimate the loss of charge to see what wall law or turbullence modelling to use, and that's the reason for the pipe without the valve. Thank you for your time and please forgive my poor english. Samuel

 December 31, 2001, 06:23 Re: Flow in pipes #2 Michael Malin Guest   Posts: n/a The Smagorinsky formulation implies the use of LES to represent the turbulence rather than the use of a statistical turbulence model plus wall functions. Are you doing LES or turbulence modelling?

 January 1, 2002, 15:37 Re: Flow in pipes #3 Samuel Calabrés Guest   Posts: n/a As far as I know, I can model the turbulence with the Smagorinsky formulation, wich implies the use of LES, but I thougt that besides there was also needed a wall law to take in account the loss of pressure due to the roughness of the pipe. Do you mean that with the use of Smagorinsky (or any other model of turbullence) there is no need to apply a wall law over the pipe?

 January 1, 2002, 22:24 Re: Flow in pipes #4 Thomas P. Abraham Guest   Posts: n/a Hello Samuel, For using LES for the Reynolds number you are looking at would need a very huge mesh. In LES, the large scales (which are anisotropic) are computed and the small scales (which are isotropic) are modeled. The model you are referring to is meant to model the small scales. Getting a mesh which would resolves the scales down to the isotropic scales would be too expensive. To make things worse, the simulation is going to be an unsteady one. Then, you need to worry about proper inlet and outlet boundary conditions to get the accurate turbulent statistics in the region of interest. It is important to note that the numerical techniques generate most of the errors at the small scales. You are better of trying a 2-equation model like the RNG version of the k-e model with wall function (this is a standard feature in most of the commercial codes today). In this case, you would be solving for the mean flow, which is good enough for engineering applications Good Luck, Thomas

 January 2, 2002, 06:00 Re: Flow in pipes #5 Michael Malin Guest   Posts: n/a My question amounts to asking whether you performing a unsteady 3d calculation using the Smagorinsky model to model the sub-grid scales (LES), or are you performing a steady 2d calculation using the Smagorinsky's model for closing the unknown correlations representing the turbulent fluxes of momentum? If it is latter, the approach is wrong and as Thomas suggests, you should use a statistical turbulence model, say for example, the standard high-Re form of the k-e model plus a logarithmic wall law using Jayatilleke-Nikaradse "sand-grain" roughness.

 January 2, 2002, 12:58 Re: Flow in pipes #6 Samuel Calabrés Guest   Posts: n/a Then I was a bit confused with turbullence. I thought that the Smagorinsky was more or less the same than the k or the k-epsilon formulations, but both the lasts use differential equations to model and the Smagorinsky uses empirical results to do the same. Thanks for the answers, Thomas and Michael. I will try with the 2 equations plus wall law as you say. Samuel

 January 3, 2002, 11:57 Re: Flow in pipes #7 Norma Guest   Posts: n/a Hi Michael, Why a 2D axisymetric unsteady simulation of a pipe flow using Smagorinsky model shwon wrong results ? Please forgive my poor english Thank you, Norma

 January 3, 2002, 12:24 Re: Flow in pipes #8 sylvain Guest   Posts: n/a Far before being used to modelize the viscosity effect of unresolved scales for LES, the Smagorinski model was dedicated to compute a turbulent viscosity used to close the RANS equations throught a Boussinesq assumption. Some CFD codes, like pamflow, still used it that way. So Smagorinski model doesn't necessary mean LES. Regards, Sylvain

 January 3, 2002, 12:51 Re: Flow in pipes #9 Michael Malin Guest   Posts: n/a Strictly, Smagorinsky's model should be used in LES, and Prandtl's model in statistical turbulence modelling. The two models look very similar except that Smagorinsky's model employs the local mesh size, whereas Prandtl's model uses the mixing length.

 January 21, 2002, 17:01 Re: Flow in pipes #10 Samuel Calabrés Guest   Posts: n/a In fact, I used the k-e model at first with Reindhardt wall law, but the results where not reallistic (in some of them even the model didn't converge). Then I tried the Smagorynsky without wall law, and the results where OK. So I think my code is the kind of that you where saying. One important result of this little study is that the velocities obtained near the valve (a floodgate one) for a little grade of opening are on the range of 70-90 m/s, with a loss of pressure of near 1 KPa. This mean that maybe there is cavitation in this zone. For more opened, there is not such problem. Thank you again to everyone and is a pity I can't put here a jpg with the results so that you could see them.

 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 kevin FLUENT 8 August 11, 2015 13:00 SMM STAR-CD 0 September 5, 2011 22:08 metro OpenFOAM Running, Solving & CFD 0 August 11, 2010 03:34 ib FLUENT 1 March 26, 2007 13:11 pxyz Main CFD Forum 37 July 7, 2006 08:42

All times are GMT -4. The time now is 10:30.