
[Sponsors] 
May 28, 2009, 23:36 
LES of highly heated pipe flow  incorrect results

#1 
New Member
Michal Hradisky
Join Date: May 2009
Location: Salt Lake City, UT
Posts: 2
Rep Power: 0 
Hi,
I’m trying to solve a flow through a vertical pipe with significant heat transfer using LES in Fluent 6.3.26. Just to give a few key parameters about the problem, Re ~ 6000 (Ucenterline ~ 5.5 m/s), D = 2.5 cm, L = 12D (with entry length, LE = 5D with constant wall room temperature, next length of 2D as a buffer, also with constant wall room temperature, and the last 5D with constant heat flux of 2200 W/m2). The working fluid is air, with all properties (Cp, thermal conductivity, viscosity) as functions of temperature, with density being set to incompressible ideal gas law. I’m using Dynamic Smagorinsky SGS model with Dynamic Energy Flux. Also, I’m using the noniterative time advancement scheme with fractional step for PV coupling, and pure central differencing schemes for both momentum and pressure, with PRESTO! for pressure. Furthermore, I’m using pressurebased solver. For the inlet I’m using velocityinlet; however, the velocities are mapped through UDF from the end of the LE section to create and “infinitelylong” entry region. The turbulent fluctuations are sustained. (The buffer region of 2D is there so the velocities at the end of LE are not ‘polluted’ from the downstream heat flux section when they are mapped back to the inlet.) For the outlet, I’m using outflow BC. The results for the initial LE of 5D are great in comparison to other LES studies of nonheated pipe flow. However, the trouble starts in the heated section. The wall temperature starts to rise, as it should, but it does not sustain the constant linear slope associated with constant heat flux flows and it drops off toward the outflow. The r+ ~ 0.3, theta+ ~ 10, z+ ~ 20, CFLmax ~ 0.1 (with dt = 2e5 sec) for the fine grid, so I hope the grid is well refined and the time step is small enough as well. I have tried all SGS models (Dynamic SL, KET and WALE) with various grid sizes and various time steps and they all seem to suggest the same trend, where the linear slope in the heated region is not sustained (from the RANS v2f solution, which is used as the initial guess and which is the only RANS model to correctly predict the wall temperature profile). I also tried using Fluent’s build in inlet perturbation techniques (Vortex and Spectral Synthesizer), but these greatly overpredict the wall temperature due to incorrect velocity fluctuations normal to the wall. I have also tried using bounded central differencing methods for momentum and energy with pretty much the same results. I have read in some forums that outflow BC should not be used for flows with strongly varying temperature (such as this flow) but instead, pressure outlet should be used. Currently, I’m trying this method, and I extended the pipe a few diameters past the original outflow at the end of 12D to ensure that vortices are still present at the end of the 12D section. So far the results do not look promising, but I have to run it for a few days to make sure statistically steadystate is reached. But in the meantime I was wondering if anyone has any suggestions or experience solving these types of flows using LES and can point out something that I’m missing or doing incorrectly. Any help would be greatly appreciated. Thank you for your time in advance, Michal 

May 30, 2009, 11:52 

#2 
Senior Member

Hi Michal,
i'm involved in some tests of the Fluent LES module. Except for the fact that you probably mean just PRESTO! for pressure and not the centered scheme which is not available for the pressure, your settings seems good for an incompressible flow. The grid and timestep parameters are good (in fact a main issue comes from the time step and even if the solver is implicit a smaller than 1 CFL is actually needed to obtain time accurate results). Could you provide the biggest values for the grid spacing in the finest grid? They are equally important in an LES and too big values could be driving some mechanism in the core of the flow. Moreover, have you tried to obtain an isothermal solution before switching on the heat transfer? This could be causing some troubles to the incompressible solver. Finally, what kind of time averaging are you performing and what kind of reference results do you have (experimental, computational)? 

June 2, 2009, 19:46 

#3 
New Member
Michal Hradisky
Join Date: May 2009
Location: Salt Lake City, UT
Posts: 2
Rep Power: 0 
Hi Paolo,
Thank you very much for your response. Yes, you are right. I meant to say that I’m using pure central differencing (CD) for both momentum and ENERGY, not pressure (which uses PRESTO!). Before choosing the time step I estimated the Kolmogorov time scale from a keps simulation of the same problem to be on the order of 3e4 seconds. Thus, to properly capture the amplitude of any fluctuations, I decided to go with dt of 2e5, which, technically, should give 15 sampling points within each Kolmogorov time period. (There is one possible problem here, the keps simulation overly underpredicts the wall temperatures. Thus, it could be that the Kolmogorov time scale estimate isn’t all that good.) I’m also running a simulation with dt of 5e6, but I have very limited computational resources, thus, this simulation is taking forever to run. As for the biggest value of r+ in the radial direction. I checked, and it starts from ~0.3/0.4 near the wall (with 5 points below r+ of 5), and the maximum spacing between two consecutive points in the radial direction (dr+) is about 11.6. The radial spacing is such there is a single point in the center of the pipe. The spacing is constant in the theta direction (100 points) and constant in the zdirection (axial direction) of dz=0.0010 m. I was mistaken on my theta+ values. Near the wall, the theta+ value (or r*dTheta+ max) is ~17 (instead of 10 as I wrote), and near the center, r*dTheta+ min is 0.03. The z+ of ~20 is correct. I know Fluent suggests theta+ max to be ~15, and z+ ~50, so my theta+ max is a little higher, but my z+ is way smaller (but because of such a high heating rate, it still may not be small enough). My solution strategy has been to start with a RANS (generally v2f) model with high heating rates already. After sufficient convergence, I switch to LES with Dynamic SL SGS model with Vortex inflow perturbation method, and after a few throughflow times, I switch to my UDF with the generator. And then I just let it run. I do not start with isothermal solution. I tried that once, but it turned out to be too computationally expensive to reach statistically steady state (SSS). But I presume, if I were to start with the isothermal solution and obtain SSS, and then turn on the heat flux boundary and get the same result as I get now, I would know that it is (or is not) the incompressible solver. As for the time averaging, right now I just use Fluent’s buildin data sampling, with sampling interval of 1 and I reset it from time to time (until I obtain SSS  so when the quantities stop changing I collect samples for a longer time period). But until I obtain SSS, I keep resetting the average with each job I submit on the cluster. I have my own routines that I used initially to do averaging, but I got the same results as Fluent. Generally, I average all results axially, because of the problem boundary conditions. That does reduce the computational time a bit. For comparison, mostly I use results from the v2f model. I have experimental data for a similar pipe flow with such high heating rate, but the pipe is ~45D long, so any LES would be way too expensive to do. But the v2f model predicts the wall temperatures for this long pipe pretty much dead on, so I use results from the v2f model for the short pipe with similar heating rate as the main comparison for my LES results. I know DNS would be much better, but I’m fairly confident about the v2f results, as far as the wall temperature goes. The one unexplored area in my research and something that I'm always wondering about is if there could be an issue with Fluent’s implicit filtering and/or the order of truncation error vs. the accuracy of the SGS model, especially since I’m using only second order methods. Do you have any experience with this? In the meantime, I’m still waiting for my results from the pipe with pressure outflow boundary condition and I also started to create a new grid for the pipe with its center section grid being square (thus, it does not have any radial consistency throughout the domain in the radial direction) and slowly transitioning to a radialtype mesh toward the wall. This new grid thus will not have any really slender mesh elements near the center, but hopefully nice and square elements. I don’t know if it is going to change any results, but, as you mention, there could be some inconsistencies in the core of the flow. If you, or anyone else, have any other ideas, I would love to hear them. Once again, thank you. Michal 

June 3, 2009, 05:00 

#4 
Senior Member

Hi michal,
from my experience your solution settings are good for incompressible isothermal flows. You're probably using a Boussinesque approach to force your flow upward and this could be an issue when temperaturedependent parameters are used. However, even if this is not the case, i'm expecting that because of the costant heat flux at the wall and the following rise in the temperature, the "+" values will begin to rise in the heated section of your pipe so you should also check that those values will still be in a feasible range. From my experience, a less than one CFL number (0.1), while providing a wellbehaved 2nd order in time convergence, is such that the time integration implicit filtering is not interfering with the space filtering, so your time step should be ok in any case. An interesting but difficult to perform check is the realization of the energy spectra for the flow in the isothermal part of your domain to see if everything is fine at any resolved scale. I did it for my incompressible channel flow at Ret = 180 and i founded that CFL = 0.9 is not enough to perform LES in Fluent because there was an inconsistent increase of energy at some frequencies (not the highest resolved ones). Even if you can't perform this check or the isothermal one, maybe some information can be gained watching at the velocity and stress profiles in the isothermal region of you flow. You should obtain the log profile and so on(after averaging). Moreover, the velocity and pressure ranges are also a good check for the incompressible solver, as well as the temperature ranges in the case of a Boussinesque approach (even if this is not probably your case because your temperature seems to not rise enough). What kind of values are you monitoring to detect the SSS? This could not be an issue in your case because your flow is developing in the axial direction so few flowthrough times should be enough but different axial stations will need different times to reach the SSS. In any case, because of the reentering approach you're using (via UDF), you need to wait at least that the flow is SSS in that part which is actually periodic and this could require more than few flowthrough times. However, axial averaging doesn't seems to me a consistent choice because your flow is not homogeneous in that direction; the only homogeneous direction in your flow should be the tangential one but the averaging in that direction is not easy (but if you have your routines you probably did it already). If the RANS results you are comparing with are believed to be correct this should not be an issue, however RANS and LES are not expected to give strictly the same results. This makes me think of a possible issue: have you turned on/off the viscous heating in the viscous model panel? Maybe i'm wrong but there could be differences in the way it is treated in RANS and LES computations. Actually, i'm expecting a strong dependence on the RANS model in RANS computations and a strong dependence on the resolved part of the flow field in LES computations. I know it's much harder (and time consuming) to do than simply say, but you could perform some checks on this term. I think it should be turned on for LES computations but i'm also expecting that this term is strongly dependent on the scheme used for the convection and the actual resolution achieved on your grid. Finally, the way in which Fluent performs LES is the biggest issue. It is a matter of minutes to write down the Finite Volume Equations for the Incompressible Navier Stokes Equations and put them in a form which is consistent with the Implicit LES. The result is definitely different from what is performed in Fluent. While this give rise to several error terms of second order which are simply disregarded (because of the second order accuracy of the flow solver), some issues still remains: 1) All the models perform in the same way with no appreciable difference in any quantity. This is because they are second order and somehow covered by the second order error of the solver 2) The dynamic procedure, as it is based on the wrong equations, is completely wrong in its implementation. In fact it is derived as if it was performed in an explicit LES computation. This error is second order too. The best way to perform incompressible isothermal LES in Fluent seems to be with unbounded centered schemes and a dynamic smagorinsky model to provide the dissipation when it is needed. Sometimes there could be stability issues connected to the centered scheme, in this case a bounded central scheme is the only feasible choice but the model is no more of any help (in this case just use the laminar option) because it is completely covered by the dissipation of the scheme. However i don't know if this is still the case in heat transfer problems and some tests should be performed. 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Pipe flow with obstacle  HELP  Min  FLUENT  6  January 31, 2017 15:28 
Gas flow in vortex tube  LES and grid resolution  bernarde  Main CFD Forum  1  March 26, 2009 11:50 
Pressure Drop  Please Help  Simple Pipe Flow  Joe A.  FLUENT  2  April 23, 2007 07:50 
LES on two phase flow  Li Yang  Main CFD Forum  0  May 12, 2004 08:10 
Hydrostatic pressure in 2phase flow modeling (long)  DS & HB  Main CFD Forum  0  January 8, 2000 16:00 