Dear "Gurus"

I am trying to solve N-S equations in CONSERVATION form for a flow over flat-plate in 2-D.

I am using Mac-Cormarks predictor-corrector methos with finite difference.

My delta_x and delta_y are in the order of 10^-8 and time-step viz. Delta(t) of the order of 10^-21. Are these values seem ALRIGHT.

The problem is.. The values spread tooo slowly in towards the internal grids. Suppose i have taken velocity at boundary to be 1300 m/s I find that only the points near boundary are affected and that to in a very slow and SMALL manner.

Really speaking.. the very internal grid points are TOTALLY unaffected!

So i increased the time-step .. but then soln goes unstable. Shall i put number of iterations very high and time-step viz. Delta(t) very small?

Thank you

Yogesh

i guess so. it is natural that with an explicit scheme and a small grid you will have to use a small time step to obtain converged solutions. you haven't said how many time steps you're using. if you'd like to converge faster you may need to find a way to coarsen some/ all your grid or use a different algorithm. otherwise run it longer

Sir,

Can I do like this. Initially use very small time-steps for some adequate number of iterations . Then use the out put of this programme as a input for the new programme which will use higher value of time-step ... I think initially its better to do it mannually as i am just a beginner.

Currenly I am using grids of 70X70 points with 1,00,000 itreations and time-step of the order of 10^-21

I hope it works... I don't know how much time it will take as i am using a simple Pentium with linux o/s.

Thank you

Yogesh

I dont know how you arrived at the figure of 1e-21. I would suggest that you use the maximum time step allowed by stability considerations. If you are interested only in the steady state solution, you can use local time-stepping. Do not stop your code by counting the number of iterations. The correct way is to calculate some measure of residue, say (rho(n+1)-rho(n))/deltaT, square it, sum over all points, divide by number of points, and take the square root. You can normalise this by dividing by the initial residue. Then run the code till this normalised residue falls to say, 1e-6. That should be good enough.

The grid is an important factor while doing viscous computations. Is your grid fine enough near the walls? The grid spacing should be based on some measure of boundary layer thickness. Try the following website which has a "viscous grid spacing calculator". It might help you.

The website of "viscous grid spacing calculator" is: <a href="http://geolab.larc.nasa.gov/APPS/YPlus/">http://geolab.larc.nasa.gov/APPS/YPlus/

Z. Lei

Based on the cfl-restriction for a one step backward euler scheme I would approximate a characteristic time step by dx/speed of sound (if u is to neglect in the boundary layer). Using dx=10^-8 gives a characteristic time step of the order of 10^-11 to me. You choose 10^-21. EVen with local timestepping one needs thousands of iterations with an explicit scheme to converge, if you are at the stability limit. For one characteristic time step YOU take about 10^10 timesteps. Multiply this by the order of 10^4-10^5, which should give an idea of timesteps you need with dt=10^-21. In otherwords: It will take forever in my opinion. You MUST have an idea of the stability limit.

wow that is many interations. however you shouls note that even with 10e6 time steps your elapsed time for the simulation is only 10e-15 of a second. do you really expect something to physically happen in that time. perhaps you could try acceleration technique like local time stepping and/or preconditioning ( i assume the problem is incompressible or at least low mach number). otherwise only coarser grid or different numerical scheme can help you use higher time step

yes it does seem as though his timestep is much too small. also i think his grid is too fine. also i think his algorithm is not the best. for boundary layer he migh want to use preconditioning and/or implicit scheme

Further, if the spacing in x-direction is also 10^-8 and you use 70 grid points in x-direction you still just cover an extremely small domain near the leading edge of the plate. But near the beginning of the plate, the exact blasius solution you might want to compare to is not valid anyway, just a bit further upstream, since the similarity parameter is not well defined at x=0.

You also have to find out how thick your boundary layer will be at the end of the plate and adjust the spacing and number of points to this. Without a knowledge of the boundary layer thickness you expect it is hard to set up a proper grid. Just guessing and hoping is not the best choice.

With a solely explicit scheme without multigrid you won't be able to compute any more sophisticated problems in any reasonable time anyway. The flat plate is usually just a testcase for validation, but not much more.

Gurus

I am trying to solve compressible VISCOUS flow in 2-D. I am using Explicit Mac-Cormrk's technique.

I am using a grid of size 72 X 72. Length of the plate is 0.00001 meter. Reynolds number is 1000. So dx=dy= 0.00001/72. Prandlt number = 0.71.

BOundary Conditions:

Flow is from left to right on the plate.

At the leading edge (Grid [1,1]) no-slip condition is applied.

At the verticle input edge i.e. left edge horizontal velocity is at Mach no. 4 and verticle direction velocity is zero. Pressure (101325 N/m^2) and temperarure (288.16 K) are at Sea level.

At opposite edge (oposite side of the plate) same condition as above is maintained.

At the surface of the plate no-slip condition is applied. And temperature is sea level. Pressure is extrapolated fron internal grids.

At the rightmost edge all quantities are extrapolated from the internal grids.

------------------------

Acording to J.D Anderson 's book it should converge after abt. 5000 iterations and problem can also be solved using 40 X 50 grids.

Yesterday i tried for 10^5 iteration with time-step = 10^-21 but the soln went unstable after abt. 5000 itreations.

I THINK THE MAJOR PROBLEM IS WITH THE GRID-SIZE AND TIME -STEP ONLY!

ANYWAY... THANKX A LOT FOR A LOT OF ADVICE AND SHARING YOU KNOWLWDGE WITH ME!

THBKX ONCE AGAIN

YOGESH

Forgive me if my comments make you uncomfortable. In order to help you out of the your problem, you need to have a basic understanding of what you are doing. (1).Your plate of 0.00001m is a very unrealistic number. If you realy want to model that tiny plate (more likely a cross-cut wire), you may want to use non-dimensional approach. (2) The Re number (if based on M=4 and L=0.00001) is too high such that you may not see any boundary layer within that small distance, or the boundary layer may not be well developed. (3) For supersonic inlet flow, you should keep a small distance between your inlet boundary and the plate leading edge. Generally, there is a weak shock wave right at the plate leading edge due to the a sudden increase of the boundary layer displacement thickness, even the plate has zero thickness. (4) You may want to use clustered grids (finer grids near the plate and leading edge, geting coarser and coarser up- and downward). (5) You time step is too small (someone has pointed this to you!) A very rough analysis gives you a safe DT about 1.0E-11. (6). Check your coding, if you run inviscid flow over zero-thickness flat plate (turn off the viscous terms), your should get very small residual at the first time step and it should not increase as time goes on. (to do this, you need to setup initial conditions to be uniform and equal to the incoming flows). (7) Do some analytical studies to get an idea of the flow field before running any CFD code.