I am not sure to understand your problem and the figures... If you are solving incompressible flows, it makes sense to speak only of pressure gradients rather than a value of the pressure at the outlet.

However, pressure gradient is unsteady and has pointwise values. To get a change in the sign of the streamwise velocity you should consider the more general balance between acceleration (eulerian and convective), pressure gradient and diffusion.

Have you tried to use Neumann conditions for the pressure at the outlet?

Is the flow rate at the outlet equal to that of any other section?

Thank you for your quick reply. For the figures it illustrates opposite behavior of the pressure gradient between 2 different time steps.

Relative to the problem , it's simple channel with generated velocity at the inlet , it suppose that the flow go from high pressure at the inlet to the low pressure at the outlet but the problem that in some time steps I found different behavior for the pressure gradient as the attached photos

1) the pressure gradient goes some times withe (-ve) and some times with (+ve).

2) from the visualization and the output files there is no velocity with negative values even at the inlet or the outlet

3)If I specified Neumann conditions at the outlet for the pressure what I have to specify for it at the inlet as already I specified the inlet velocity???

4)the flow rate is slightly change between the inlet and the outlet such as at inlet U= 0.199937 and at the outlet U = 0.20022 and the same range for all time steps.

If you are performing a DNS or LES case, the streamwise component in the outlet plane must show some locations of negative velocity due to the vortical structures in the boundary layer.

Then, I do not understand if your plots are ensembe average of the pressure, you should consider that only in the statistical averaging you can get the expected pressure loss.

As the BC.s are concerned, you prescribe Dirichlet for the velocity and Neumann for the pressure at the outlet, right?

At the outlet, you can use the convective condition for the velocity and then prescribe the Neumann condition for the pressure.

Check better the difference in the flow rate, it should be lesser than what you get.

Dear Filippo,

Sorry to be late for the reply as I was out of office for work. I'm using LES in OpenFOAM. In the cases which I run all the streamwise components at the outlet are positive, I'm not sure if this right or not.

I specified for the pressure at the inlet as zeroGradient and the outlet as a fixedValue (0) (Dirichlet B.C) and for the velocity I applied my generated B.C at the inlet and Advection one at the outlet.

In that case as for unsteady channel flow, can I neglect the instantaneous pressure behaviour and work only on the Mean pressure values?

I checked them again and you were right the inlet is slightly higher the outlet not the opposit

In an LES of turbulence, the flow close to the wall (i.e. the turbulent boundary layer) is highly separated and unsteady, therefore if you do not see that in the outlet plane, something is wrong. Maybe your SGS model is too dissipative and tends to re-laminarized the solution?

COuld you show more details and plots of your solution?

I'm using WALE as a SGS model and from the review it was the most suitable one for turbulent B.L in a channel flow. So, Could you please tell me what details and plot I have to show it?

I would definitely adopt the dynamic model. However, have you ensured the correct grid resolution close to the walls? The flow is homogeneous in spanwise direction?

You should plot the velocity at the inflow plane and along 2-3 planes along the streamwise direction until to the outlet plane. Of course, only at a time when the flow is fully physically correlated

It could be very useful if you compute the total kinetic energy in the domain versus the time.

I put the mesh near the wall to be fine with y+=0.3. So what do you mean by the flow homogeneous in the spanwise , if you are talking about the velocity profile so the answer will be yes. if you are talking about the fluctuations not identical. but at the inlet the generated fluctuation is homogeneous and the mean velocity from a previous fully developed case with V=W= 0.

Attached here the velocity profile at the inlet , mid, and before the end of the channel. This profiles after about the flow pass through the channel with 15 times which I think it's fully physically correlated.

For "homogeneous", I mean if you are using periodic conditions in the spanwise direction.

You should plot the velocity profile u+ in terms of the y+ location to understand better the figures. What I see from the profiles is that you never get a negative streamwise velocity in the istantaneous velocity. While that is correct in terms of RANS solution, in LES you should get turbulent vortical structures close to the wall.

yes it periodic conditions in spanwise. Attached the velocity profile at the 3 positions.

According to the negative streamwise velocity, let's discuss about it, I think it's OK to get all values are positive because I'm working on attached boundary layer not separated one.

You are working at quite small Re_tau number (it seems to be less than 200 if considered in terms of the channel height), to tell the truth I am not sure if at that number you can have a fully developed turbulent BL without vortical structures...

However, the statistically averaged velocity profile at the outflow appears quite acceptable. You could compare them to the DNS profile at Re_tau=180 you can find in literature.

the used height of the channel = 0.1 m and Re_tau in the range of 500.

and the mean velocity is comparable with the DNS results which has Re_tau=500 and

delta is the half height of the channel

Re_tau= (u_tau*delta)/nu

If the scale is logarithmic, the max y+ in the plot is less than 200. That value is reached at the half-height of the channel and corresponds to the Re_tau value of the problem. Therefore, you cannot have Re_tau=500.

Otherwise your plot is cutted in the higher range...

"How can pressure at the outlet of channel flow be higher than the pressure at the inlet without any back flow?"

The flow can sustain an adverse pressure gradient if the velocity "U" that you set at the inlet is high enough. Roughly if: 1/2*rho*U^2 > deltaP, then there is not backflow. Otherwise there is.

Hi Filippo,

you are right the plot has been cut and attached here the full curve till y+ =450

Hi Martin,

Brilliant. so you mean that there is possibility to get adverse pressure gradient when the generated velocity at the inlet is high, So now I'm generating fluctuations only and UMean is constant, so at some time steps the generated fluctuations are very high which cause that as there are some time step has the normal pressure gradient. is that what did you mean????

Another thing,, Is that affects the study of the turbulence in side the channel??

How can I be sure for the time to start to take results from my run ??

Dear Mohamed, it would be nice if you could rewrite you last post properly. I am really struggling at understanding what you mean.

Dear Mohamed,

the velocity computed at the outlet is quite acceptable. I see some oscillations at the higher y+ values, are you sure that the number of samples for the statistical averaging is sufficient? Check also the RMS along y+.

Finally, since you have periodic conditions in streamwise direction, I strongly suggest to do a spectral analysis.

Hi Martin,

I was trying to illustrate my work just trying to generate inlet B.C for channel flow with specific amount of RMS at the inlet and UMean for the inlet taken from a previous fully developed channel flow with a velocity profile follow the law of wall. So, according to your comment in some time steps may be the generated fluctuations are very high which cause adverse pressure gradient. Is this what did you meant by your comment? . if yes, to what extend it will affect on the results of a turbulent B.L?

Hi Filippo,

This Oscillation may be due to the coarse mesh at the center of the channel relative to that one near wall.

it's not periodic in streamwise I've inlet and outlet B.Cs.

Attached here the urms in streamwise direction at the 3 positions of the test.

Sorry I wrote streamwise but I wanted to write spanwise direction

Just a doubt, why the RMS curves extend differently along the x axis? Do you compute differently the y+ values?

Could you superimpose the RMS of the DNS?

Actually the y+ range differs slightly between the three slices due to the difference in u_tau at each slice as I computed y+ for each slice separately depending on its u_tau for the slice For the paper which I'm trying to compare with it, it gave only the Reynolds stresses as a first step when they are identical at the 3 slices it indicates that I got homogeneous turbulence. Attached here the Reynolds stresses for the 3 slices which I got from my calculations.