CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Main CFD Forum

FLOW OVER FLAT-PLATE *again*

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   September 21, 1999, 06:23
Default FLOW OVER FLAT-PLATE *again*
  #1
Yogesh Talekar
Guest
 
Posts: n/a
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
  Reply With Quote

Old   September 21, 1999, 10:35
Default Re: FLOW OVER FLAT-PLATE *again*
  #2
clifford bradford
Guest
 
Posts: n/a
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
  Reply With Quote

Old   September 22, 1999, 00:01
Default Time-steps change*??*??*??
  #3
Yogesh Talekar
Guest
 
Posts: n/a
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

  Reply With Quote

Old   September 22, 1999, 01:58
Default Re: Time-steps change ?? ?? ??
  #4
Praveen Chandrashekar
Guest
 
Posts: n/a
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.
  Reply With Quote

Old   September 22, 1999, 04:22
Default Re: Time-steps change ?? ?? ??
  #5
Zhong Lei
Guest
 
Posts: n/a
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
  Reply With Quote

Old   September 22, 1999, 10:39
Default Re: Time-steps change ?? ?? ??
  #6
Frank Bramkamp
Guest
 
Posts: n/a
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.
  Reply With Quote

Old   September 22, 1999, 11:29
Default Re: Time-steps change ?? ?? ??
  #7
clifford bradford
Guest
 
Posts: n/a
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
  Reply With Quote

Old   September 22, 1999, 11:32
Default Re: Time-steps change ?? ?? ??
  #8
clifford bradford
Guest
 
Posts: n/a
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
  Reply With Quote

Old   September 22, 1999, 11:45
Default Re: Time-steps change ?? ?? ??
  #9
Frank Bramkamp
Guest
 
Posts: n/a
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.

  Reply With Quote

Old   September 23, 1999, 00:22
Default ALL DETILS OF THE PROBLEM
  #10
yogesh
Guest
 
Posts: n/a
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
  Reply With Quote

Old   September 27, 1999, 12:08
Default Re: ALL DETILS OF THE PROBLEM
  #11
Hongjun Li
Guest
 
Posts: n/a
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.

  Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Supersonic flow over flat plate Nikhil Main CFD Forum 6 May 20, 2013 12:48
incompressible, 2-D laminar flow over flat plate... varunjain89 Main CFD Forum 3 March 6, 2012 12:13
HELP! Flow over both sides of a plate. farocean97 Main CFD Forum 0 September 12, 2011 10:57
Flow over flat plate using FASTRAN AndyLiu Main CFD Forum 1 August 7, 2006 08:02
results for flow past flat plate normal to flow lisa Main CFD Forum 2 August 30, 2005 16:36


All times are GMT -4. The time now is 20:02.