u plus vs y plus
 

Dear all,

I have a question about plotting u plus and y plus.

I creat a line on floor with a certain height, define u plus and try to plot u plus vs y plus, but i can only get one pair data.(Based on y plus definationhttp://www.cfd-online.com/W/images/m...22904f345d.png is the distance to the nearest wall, so i can only get one pair data)

But if i want to see how does uplus vary with y plus, like the linear and the log relatoin, what should i do?

Best regards

Chne

What you want to plot is actually nothing different from the classical velocity profile in the direction normal to the wall, but in different coordinates. Hence, if you have the pairs u - y (for different values of y!), you have to plot u/u_tau vs. y * u_tau/(mu/rho), where y is the wall normal coordinate. You are probably making confusion between the y+, the transformed wall normal coordinate, and the dy+, the transformed wall normal coordinate of just the first point off the wall.

i am not so clear about you mentioned dy+(do we need this variable when plotting u+ vs u+). I mean i ploted u+ vs y+ along a line which is perpendicular to the floor,but i can only get one pair value, seems like only for the neasrest node close to the floor.
y plus is meaningful for the nearest node or for all the nodes ? If we look at its definetion , it's calcuated from the wall shear tress(U_tao=roor square(wall shear stree/density)), but wall shear stress happens on the wall. so how i can get the y plus for the rest of the nodes except for the neasrest one?

or i misunderstand something?

Probably now i get the point: if you are using Fluent to do this, it will work as you described as it has y+ defined only at the near wall cells hence it cannot give you the values all along the specified lines. However this is just a Fluent feature (mostly due to the memory saving necessity) and of course y+ is meaningful all along the wall normal direction as, for example, the wall laws are defined in terms of y+.

Actually, in fluent, you are just plotting y+ vs y which is dy+ vs y as it is given only in the near wall cell.

The best thing you can do is to export your velocity profile (u vs y) in a file and then use, say, matlab to make the coordinate transformation with the wall stress computed by fluent. The wall stress is just the value at the wall and it is obviously the same all along the line

Otherwise, i don't get why you should get just a point instead of the whole line you created

Thanks very much for your advice! Now it's clear! :)

Problem solved!
 

Sbaffini! Excellent reply of plotting the curve in Matlab or Excel. You made my day. The thing I had been looking for years is solved today. Hats of for you

Sbaffini, how are you? I hope you will help me again. Here is the problem I am stuck at:
"
I have modeled a quarter pipe with its solid thickness modeled too. I have applied the flux over wall as 3500 W/m2. I have the formula for havg= flux/(Tavg,fluid-Tinside). The T inside is the temperature at the lower end of wall, the region that touches fluid.
In experiment Tinside is measured via thermocouples that are installed across the tube length wherever the flux is applied. These TC however measures the inner temperature of the wall.
Nusselt number is Nu=havg*Di/k. Di=inned dia, and k=thermal conductivity of fluid.
My computed Nu is very low from experiment. I am using Fluent, and applied flux on top wall. and specify coupled BC on interface. This creates wall shadow.I do not use any heat value (flux or temp) except on top wall. I saw as well "via System coupling" written in these BC. do I need to turn it on too? In fluent I take Area weighted average for inlet and outlet (Ttotal) while for Thermocouples I made Isolines at TC positions and took Temp (total) with Area weighted average.

The error is more than 10 % from experiment."

Please help me as I am not able to find a solution yet.

y* is the non-dimensional distance multiplied by Re_tau, this way you can plot u*(y*) in a log plot

Dear Shamoon,

there might be several causes for your results. Unfortunately it's been a while since the last time i used Fluent.

I suggest you to first check your setup (or a similar one) against a known laminar solution (for example, the CHT problem of a laminar poiseuille flow with an external solid tube can be solved analytically).

An additional check might be to add an additional solid layer in your tube, made up of a different solid material, and adapting the b.c. to this new layer. If everything works properly, you should get the same solution in the original domain part.

If everything is ok, the problems are either concerned to the postprocessing (which i experienced in the past for the CHT) or the turbulence modeling (which is unlikely, due to the very simple geometry).

Concerning the postprocessing, the problems i had were related to the way the local heat flux was produced in output (both contours and files) for coupled walls. I finally decided to do this postprocessing by myself (actually a student i was supervising :D), by having fluent write the temperature variables in celle centers on both sides of the surface and reconstructing the actual flux from the known interpolation scheme used by fluent.

I don't know if the wrong behavior i experienced was determined by the fact that i was also using time statistics. Moreover, it was also fundamental to understand clearly what was the experimental output and how was it computed, in order to do the postprocessing in a consistent way.

Hope this is helpful.

Dear Sbaffini

I finally decided to take the interface temperature all along the pipe length and not the thermocouple locations. So error is observed at somewhat large Re . The thing you say, that do interpolation by yourself, may be I give it a try too. Strangely, the two interfaces, from which fluent creates wall and wall shadow have different temperatures. Please note that I modeled the wall thickness and meshed it as well and named the interface zones. I apply the flux on the outer side of the wall that has solid adjacent cell zone. Its very strange to me that the two interface are like two sides of a same coin and give different temperatures.
1. Could you tell me how Fluent does interpolation? Can I do it by myself?
2. Any particular case of pipe flow with wall thickness in your opinion?

Best Regards,

Dear Shamoon, in the end, in my specific case, to exactly match what was done in the experiment, i had to work from the solid side, which means take temperature and heat flux as computed from the surface (the true one or its shadow) that sees the solid as adjacent cell thread (this information is available in the b.c. panel). More over, a particular attention had to be paid to the definition of the Nusselt number, if local or average quantities were used, etc.

The other options i tested, based on interpolation, were simply based on taking the temperature in the cell center adjacent a given face on the coupled wall and the heatflux on the same side, then reconstruct the local temperature gradient dividing the heat flux by the thermal conductivity and finally reconstruct the surface temperature with a linear interpolation from the cell center (with heat_flux positive if entering the cell_center zone)

T_surface = T_cell_center - heat_flux/k * (x_surface-x_cell_center)


I tried this from both sides (fluid/solid) and also averaging them. In the end, as i said, temperstures and heatfluxes computed from the solid side were consistent with my experimental reference and worked for me. Still, each of these approaches produced different results for me :eek:.

Honestly, i suggest you to be always suspicious of the CHT results in Fluent, double check heat flux consistency among zones, etc. One of the latest issues i had was with a very simple 2D setting. Bottom solid, laminar channel, middle solid, turbulent channel with wall functions, top solid. Temperature fixed at the boundary solids, periodicity, driving source terms in the two channels. All the classical pressure based solver diverged at the first iteration (:eek::eek::eek:), the density based was unable to transmit heat among the different zones with the temperature retaining, essentially, the initialization value (:eek::eek::eek::eek::eek:), only the coupled pressure based solver produced a reasonable solution (equal temperature gradients in the solid zones with equal conductivities, as it was essentially a 1d problem) which, nonetheless, had some funny issues (a temperature discontinuity, due to the wall function and large pr of the fluid, only on one side of the turbulent channel, instead of both).

Dear sbaffini,

Thanks for your kind reply. I can try your method as well. The thing I mentioned yesterday about two different temperatures at interface was because I was taking the total temperature. However, static temp was same on both sides. Although the difference between static and total is not much.
Secondly, the formula in Nu is havg*D/k where havg=flux/(Tavg,w-Tavg,f)
Tavg,w = mean of the inner wall temperature
Tavg, f = mean of inlet and outlet
What I did was that first blindly followed the formula. I took area weighted average at 8 thrmocouple locations and noted the temperature at those stations (those were lines formed at interface).
I took mass weighted average btw inlet and outlet
Using this method gave me error range from 18-23%.
For second iteration, I took interface and took area weighted avg of total temperature. I took MWA value for second term just at pressure outlet. This improved my results. And now I am sticking to it because the experiment guys said themselves that the error in Nu is +- 18%. I am sending you some images from paper, that may be help you in understanding my prob.

Ok, one more thing, I also have to compute friciton factor. FF depends upon pressure and I put the operating as 101325 and gauge press at outlet to zero. This gives me correct pressure at velocity inlet which is infact delta p in friciton factor formula.
Problem is that even after 25000 iterations it is dropping down, but very slower rate, so at which point should I stop?

I did not understand
 

I want to plot a graph of u+ with y+ for a pipe flow (2D sketch) with Re = 10,000. I have y+ and I have defined the expression in u+ = velocity u / (sqrt(Wall Shear/Density)). However , I am getting erroneous results.
Please help.

The shear stress is the first value of wall shear stress in the first cell. It will obviously be zero elsewhere. So if you are using Fluent, go to xy plot and plot the wall shear stress on the radial line. IT will show you a maximum of wall shear stress just near to the wall. Keep node values on. NOte it down. Then use it all over for computing u+ or y+.

I am analyzing a turbulent pipe flow with Re = 10,000 with diameter of 0.2 and length of 3 m. However, due to symmetry, I analyzing for radius of 0.1 ,ie, from wall to centreline. I have written an expression as mentioned in my previous reply. However, I am not getting the results as per the log law and hence needed help. I have attached the photos of the graphs from my analysis.

Attachment 59137

Attachment 59138

Thanks in advance!!

your plot u+(y+) makes no sense, it does not vary along y+ but it has y+=constant!
First, you have to compute the Re_tau, you can then represent the plot from y+=0...Re_tau

I did not understand. How to proceed further ?

y+ is nothing else the a local Reynolds value, going from 0 at the wall up to Re_tau at the centerline. U+ is scaled by u_tau. Then you have to plot your u+ along y+. Therefore, you have to use the proper normalization and you grid law along y.