Hi,

I'm currently trying to verify my code using the bfs example. I', using a 2D fully implicit FVM fractional step code by Kim & Choi (JCP 162 p411).

My domain is a rectangle domain 30h X 2h. A parabolic velocity profile enters left of domain at y=1h to 2h. Other initial conditions for velocity and pressure are all zero.

I'm not too sure about the boundary conditions though, mainly the inlet & outlet.

For left BC, u= parabolic profile, v=0 from y=1h to 2h u=v=0 for y=0 to 1h dp/dn=0 from y=0 to 2h

For outlet BC, du/dt+Uc*du/dx=0 and dv/dt+Uc*dv/dx=0, discretized as

u(n+1,i+0.5) = u(n,i+0.5) - c*(dt/dx)*(u(n,i+0.5)-u(n,i))

n refers to current(known) time step i refers to right extreme cell centered node. i+0.5 refers to right extreme(boundary) face location c = space-averaged streamwise exit velocity

p=0 at outlet.

May I know if this is correct? Thank you

Hi !!

These seems to be correct, if you are using them with the no-slip bc's at the top and bottom boundaries. Many good references are available for this problem with bc's.

Regards, ramp

You'll find this benchmark problem fully described in page 95, section 8.2 of the Gila user's guide, available in http://www.prod.sandia.gov/cgi-bin/t...003/031781.pdf

Another very good reference is the book of Michael Griebel, Thomas Dornseifer and Tilman Neunhoeffer, "Numerical Simulation in Fluid Dynamics - A Pratical Introduction" SIAM, 1981 ISBN 0-89871-398-6

Cheers

Renato N. Elias High Performance Computing Center NACAD/COPPE/UFRJ http://www.nacad.ufrj.br/~rnelias

Oh ok thanks. i've also managed to get the reference by Armaly, which is same sort of benchmark.

however, my ans still diverged, esp. the top left corner, using 100*40 cells

I'm still not very sure about the pressure boundary condition, which is required since I'm using colocated grid.

I'm quite certain that at the top/bottom walls, dp/dn=0 Most references have given p=0 at the outlet.

So what about the inlet? should it be dp/dn or p = 0?

Thanks again everyone.

Hmmm, I've ran this benchmark problem once in the program that I've developed in my MSc. The solver was based on a finite element method (SUPG/PSPG formulation) using triangules to solve the steady incompressible Navier Stokes. The kernel of the computation employed an inexact Newton-GMRES running with 0.99 as initial linear tolerance (the inexact solver chooses the linear tolerance adaptatively). I've employed the following boundary conditions to run examples with 100, 250 and 500 Reynolds numbers

inlet: velocity = (1,0,0) walls: velocity = (0,0,0) outlet: pressure = 0

the results were good according to those described in Griebel's book.

Regards

Renato N. Elias High Performance Computing Center NACAD/COPPE/UFRJ http://www.nacad.ufrj.br/~rnelias

Check you code with the following specification. I dint find any convergence problem with these bcs and grid etc.

L=20h, H=2h where h: is step height. Grid size: 120*60 for Re=133, 267, 400 and 600.

B.Cs:

Inlet (x=0)::

u=6y(10y), v=0, dp/dn=0 for y=0 t0 (H-h)

u=v=0, dp/dn=0 for y=(H-h) to H

Outlet (x=L)::

du/dx=dv/dy=0; p=0 for y=0 to H

Top and bottom (y=0 and H)::

u=v=0, dp/dn=0 for x=0 to L

hi, ramp, is there a mistake in your BC?

Assuming y increases downwards,the inflow does not has a parabolic profile. Does it matter?

at outlet, should the BC be dv/dy=0 or dv/dx=0?

it was given as dv/dx=0 in Armaly's paper.

I'm now trying a simple 2d duct flow with uniform inlet velocity and p=0 at outlet. However, the ans still diverges. I'm still trying to find the bugs .....

Thanks

Sorry quarkz, its dv/dx not dv/dy

The parabolic profile is just a assumption that the flow at the inlet is fully developed and the flow must be fully developed at the point of expansion.

Well, I've implemented the BCs and initial conditions as suggested by ramp. I'm now doing a very simple case of uniform inlet velocity, developing into a parabolic velocity profile at the outlet.

initial conditions are u=1. at inlet. the rest of variables (u,v,p) are 0.

After 0.01 time, the velocity vector plot looks ok except for large velocities at the 2 inlet corners. It gets worse as time proceeds and this is the main prob.

I' wondering what could be the mistake... could it be the outlet BC (something to do with reflecting BCs?)

NB: is there a need to come up with divergence free initial conditions? I just set u=1 at inlet, the rest v,p are zeros....

thanks alot!

Well, maybe someone who've encounter this before can help...

I'll transcript what is written in page 76 of Griebel's book about the initial condition of the backward facing step.

"When setting the initial values of u it is useful to only set u_0 = 1.0 in the upper half of the domain, leaving u_0 = 0.0 in the lower half. This ensures that the initial veloticy satisfies the discrete continuity equation."

In the same book the inlet velocity is set to 1.0 uniformly (not parabolic)

Cheers

Renato N. Elias

Hi !!

Why dont you check a case of flow inside channel... Use the uniform velocity at the channel inlet, rest all boundaries similar to earlier and let the flow to be fully developed. In this case, you know the entry length (Le=Constant*Re) for a particular Re and check whether the flow is flow developed near about the length (Lx =~ Le) or not. If eveyrthing is in order then you must get them approximate to each other. Check the flow at low Re, so that you can validate the things in short time.

You can use initial conditions as zero for u,v and p.

Renato, I dont have copy of this book but I think they might have taken the inlet velocity as 1.0 and the length of channel before the expansion zone to be sufficient enough for flow to fully developed.

The idea of using parabolic velocity at the inlet is to save the computational time because If you solve the flow with the uniform velocity then you should have extended domain before the point of expension which is sufficient enough for flow to be full developed and this length of the domain (entry length) will vary with the Re. And so if one want to reduce the computational time then should apply the parabolic profile at the inlet (which is point of expension).

Best regards, ramp

Yes Ramp, you're right. I was just transcripting what was written in the book regarding the uniform inlet velocity, but, I've already ran this problem in 3D with the same inlet condition up to Re=500 without any problem. I think it's more straightforward to set up uniform inlet BC than to calculate a parabolic profile.

Regards

Renato N. Elias

thanks ramp & Renato!

i've tested on a flow inside a channel. the problem is the high pressure gradient after solving the poisson eqn, which results in very high u,v velocities at the cells at 2 inlet corners. I've managed to alleviate it by using 2nd order 1-sided dp/dx approximation to get the west pressure face values, instead of simple linear extrapolation. however, devergence still occurs after a longer while.

the only solution is to use some sort of under relaxation for the pressure as in the SIMPLE scheme. in that case, I'm able to get a parabolic profile ie the correct ans. but the unsteady nature will not be captured.

hence, i believe there are 2 problems which needs to be solved:

1. is p(west face)=p(1,j) (from dp/dx=0) a good approximation?

2. Imposing an inlet velocity as the initial conditions 'll result in a non-divergence free initial conditions. Will that matter?

Hope someone can help. thanks again

Hi !!

I guess there is some problem with your pressure calculation part. The channel flow is a simplest problem and if everything is in order, then you must get the things properly.

You can make the channel flow problem more eassier by applying the slip boundary conditions at top and bottom and uniform flow at the inlet. Use the u,v,p=0 as the initial condition. You will get uniform flow throughout the domain. If its also diverging then first check your pressure calculation subroutine.

Do you get the correct answer with any other problem (say cavity flow, etc.) with this code?

Best regards, Ramp