I am wondering if any one of you have reached the fully developed flow in a simple Pouseuille flow problem where normal velocity should reach 1.5 (i.e U/Uin = 1.5). I am using velocity BC at the inlet and 1st order extrapolation BC in the outlet. My results give 1.4 instead of 1.5.
The second question is that when I used 2nd order extrapolation the velocity profile reduced to 1 although all other things are fixed. Also, how about the value of the density at both inlet and outlet sections? Do we need to keep it close to the initial value and for what percentage? If it increases rapidly but with nearly fixed gradient would that be acceptable no matter what the final value is? Suggestions are highly appreciated.

By the way, I tried three values of aspect ratio 10, 20, and 30. Non of them produces the value of 1.5 fully developed flow although the velocity vectors look very nice.

I do not understand your first problem completely. Since you are talking about an aspect ratio: Do you perform a 2D or a 3D-simulation? Do you start with a constant velocity profile on your inlet? Exactly what kind of velocity BC do you use? What is your lattice resolution?

I am using D2Q9 model. I started with constant velocity profile at the inlet (U[sub]in[/sub]=cons) to setup the initail values. I am using Zou and He velocity BC. The resultions of the lattice are 600x60, 1200x60, and 2400x80 respectively.

what is your Reynolds number? For not too large numbers (Re < 10) you should reach a fully developed flow after 1 or 2 L lattice nodes, where L is the diameter of the channel. Since your aspect ratio is much larger, the flow should be fully developed at the middle of the channel, unless you have a crazily large Reynolds number.
I assume that either your code is not working correctly or the implementation of the boundary conditions is wrong.

The Re number that I use starts from 400 and larger. Yes I got the fully developed shape of the velocity profile but it is not totally fully developed (U/uin=1.4 insted of 1.5). I was willing to show you my results yet I do not know how to post it on this page.
If you give me your email I will send it to you

a Reynolds number of 400 is not very small. For this value you should take an aspect ratio of at least 50 in order to have a fully developed flow at the middle (in flow direction) of the channel. That may be the reason why you do not observe the correct factor of 1.5.
I suggest the following: Either reduce your Reynolds number by a factor of 10, say, or increase your aspect ratio accordingly. There is a nice paper on the required development length for a fully developed flow by R. J. Poole and B. S. Ridley: “Development-Length Requirements for Fully Developed Laminar Pipe Flow of Inelastic Non-Newtonian Liquids”, published in “Journal of Fluids Engineering” (October 2007, Volume 129, Issue 10, pp. 1281-1287).
If this does not help, you can give me your results (I send you my mail via PM).

The problem suggested by Alam is very interesting. If you drive a fluid through a 2D channel by enforcing a constant velocity uIn at the inlet, the flow approaches asymptotically a Poiseuille profile, far from the inlet. The maximum velocity at the center of the parabola is then given by uMax = 3/2 uIn, independently of the Reynolds number. This is easily verified if one assumes that, in an incompressible regime, the integral of velocity along a cross-section of the channel is constant, i.e. independent of the position in the channel.

I think however that one needs to be careful about boundary conditions in order to verify this property numerically. On the inlet, imposing the velocity uIn on each node may not be sufficient. From the argument above, it is clear that the only really important constraint is on the total amount of injected momentum. Take the example of a channel width of four lattice nodes. Throughout the channel, node 0 and node 3 are Zou/He boundary nodes which implement a no-slip condition, and node 1 and 2 are fluid nodes. In that case, the channel width is L=3 in lattice units. Thus, the integral of velocity over the inlet should yield LuIn in lattice units. Numerically speaking, this means that the sum of the velocity over each inlet node should be LuIn=3uIn. If only node 1 and 2 on the inlet have velocity uIn, then your sum yields 2uIn which is too little. If node 0 and 3 also have velocity uIn, then your sum yields 4uIn, which is too much. Therefore, I would suggest to impose the velocity 3/2uIn on node 1 and 2 (or in general L/(L-1)*uIn on each node except the two wall nodes), which yields the proper sum.

Attention: this argument is invalid if you used full-way bounce-back instead of Zou/He for the channel walls. In that case, the channel width in our example is only 2 instead of 3.

I agree with Timm that you are better off starting with low Reynolds number, to avoid exceedingly slow convergence rates. Also, if you experience problems with a Neumann outlet condition, it would be interesting to try a pressure condition on the outlet. With Zou/He boundaries, it is easy to impose a fixed density (say, rho=1) at the outlet.

Some days ago I have tested my code (D3Q15) by using a constant velocity boundary condition (regularized at inlet and outlet) on a 3D channel with 20x40 lattice nodes cross section. The boundary condition on the side walls was full-way bounceback. I used the Reynolds numbers 2, 6 and 18. In all cases I have reached a fully developed flow after some time. The mean relative deviation from the theoretical profile was 0.35 % for Re = 2. Actually, this deviation is smaller as the one obtained from a simulation with periodic boundary conditions and a constant body force under the same conditions.
My result: The velocity boundary condition is working very nicely in three dimensions.

First of all thank you for your suggestions and efforts. Do not you think that using aspect ration of 50 is to much in order to reach fully developed flow veleocity profile. For the profile I obtained it even when L/H is less than 10. My conceren is about the value Umax/Uin=1.5 which I could not reach unless some modifications are made for the boundary conditions. By the way I am using full way bounce back BC on walls.

This may rises the following question; is it ok for the density to increase rapidly (up to 6 / 7 times the original value) while the density gradient is approximatly constant? in that case I can obtain a closer value of the max velocity to 1.5 of Uin.

Regarding the Reynolds number, I think the velocity profile should reach the same value of 1.5 regardless of the Re value in case of fully developed flow. The only differences are the entrance effect and the cross section where we can obtain the fully developed flow. This is addressed in the Poole et al paper by that you mention, which is highly appreciated.

of course the fully developed profile itself does not depend on the Reynolds number, but the length after which it has developed does. That is the reason why one has to make sure that the channel is long enough. But since you state that you reach fully developed flow, the error has to originate somewhere else.

I find it strange that you have such a large mass increase (factor 6 or 7). In my simulations I usually have a mass increase / decrease of max 1 % after 50000 iterations. I think that your inlet / outlet boundary conditions are incorrect. What is your Mach number? If the Mach number is too large (> 0.1), the mass increase is very high. In my simulations I always make sure that my Mach number is in the range of 0.01. It may be possible that the pressure on your inlet / outlet lines is not correctly chosen. But I am no expert on this.

A PM is a private message, have a look at the top right of this page. But I have some problems with sending them, maybe my message did not reach you.

The problem suggested by Alam is very interesting.
If you drive a fluid through a 2D channel by
enforcing a constant velocity uIn at the inlet,
the flow approaches asymptotically a Poiseuille
profile, far from the inlet. The maximum velocity
at the center of the parabola is then given by
uMax = 3/2 uIn, independently of the Reynolds
number. This is easily verified if one assumes
that, in an incompressible regime, the integral of
velocity along a cross-section of the channel is
constant, i.e. independent of the position in the
channel.

I think however that one needs to be careful about
boundary conditions in order to verify this
property numerically. On the inlet, imposing the
velocity uIn on each node may not be sufficient.
From the argument above, it is clear that the only
really important constraint is on the total amount
of injected momentum. Take the example of a
channel width of four lattice nodes. Throughout
the channel, node 0 and node 3 are Zou/He boundary
nodes which implement a no-slip condition, and
node 1 and 2 are fluid nodes. In that case, the
channel width is L=3 in lattice units. Thus, the
integral of velocity over the inlet should yield
LuIn in lattice units. Numerically speaking, this
means that the sum of the velocity over each inlet
node should be LuIn=3uIn. If only node 1 and 2
on the inlet have velocity uIn, then your sum
yields 2uIn which is too little. If node 0 and 3
also have velocity uIn, then your sum yields
4uIn, which is too much. Therefore, I would
suggest to impose the velocity 3/2uIn on node 1
and 2 (or in general L/(L-1)*uIn on each node
except the two wall nodes), which yields the
proper sum.

Attention: this argument is invalid if you used
full-way bounce-back instead of Zou/He for the
channel walls. In that case, the channel width in
our example is only 2 instead of 3.

I agree with Timm that you are better off starting
with low Reynolds number, to avoid exceedingly
slow convergence rates. Also, if you experience
problems with a Neumann outlet condition, it would
be interesting to try a pressure condition on the
outlet. With Zou/He boundaries, it is easy to
impose a fixed density (say, rho=1) at the outlet.

Hi Jonas,

Thanks for your explanation. I am corrected the uniform velocity according to your suggestion and it works. I have few questions regarding this. Can you please explain?

I am using the following conditions for the poiseulle flow

Zou-He Uniform Velocity Inelt

Constant Pressure (1) outlet

Zou-He no-slip on the walls

Incompressible SRT BGK

I corrected the uniform velocity according to your analogy and it seems to work good. The only problem is at the inlet since I am using Zou-He on all boundaries I need to specify the corner boundaries too. And for the velocity boundary condition at the inlet there is not equation for the density at the corner and it needs to take the value from the next node. Because of this I see an y-velocity at inlet nodes. Gradually this y-velocity decreases along the channel. Is there any way to suppress this. Please explaion.

Hello Dear
Actually I have done my matlab code for Channel with Multi relaxation time but i think it has a problem with boundary condition and for example after 130000 iteration my code is crashed ,I was wondering If you could check my code and then say me what kind of boundary condition I should apply for Channel . I’m looking forward to hearing from you. Thank you for your consideration and time.