Hi,
I used sonicFoam for solving the flow through a nozzle. I encountered the same problem of diverging Courant number after a few iterations. Changing the numerical scheme for the divergence terms did solve the problem. After some time, I found that my specific heat capacity (c_v) was specified incorrectly. When I changed c_v from 1.78571 to 717.51 and started the iteration process, the Courant number did also diverge, however it is stable over many time step before it suddenly diverges. Can anyone explain this to me? |
did you just change Cv and nothing else?
if you just set up Cv and don't change R and U, then you get a completely different case. with Cv the speed of sound is defined as: c=sqr(R*p/rho*Cv + p/rho) if you just change Cv, you change c. check all other variables, possibly there is a problem. |
I changed the Cv value, only. Now, I'm sure that I defined R and Cv correctly.
After some investigation of the flow, I encountered another possible source for the diverging Courant-number. The following happens: I'm simulating a supersonic convergent-divergent nozzle. There is a shock in the divergent part of the nozzle causing the boundary layer to separate, which creates a vortice. This vortice is transported towards the outlet. When it hit the outlet, there is a sudden and dramatic increase in velocity in this region, which is pointing into the nozzle. Thus the Courant-number increases. I'm quiet sure that this increase in velocity is artificial. I suppose, it occurs because of reversed flow due to the vortice. The BC at the outlet obivously does not let the vortice pass. I already used the 'totalPressure' BC and a 'fixedValue' BC for the outlet, however, the effect occurs for both types. Can anyone suggest a BC which is more appropriate? |
ok, i never used 'totalpressure', but 'fixedValue' is wrong.
for mu=0 the sonicFoam solver solves the Euler-Equations. These Equations have the eigenvalues v-c, v and v+c. For a supersonic flow all these eigenvalues are >0 so error shocks run all in your flow-direction. So have to set 3 fixedValues at inlet and no value at the outlet. try 'zeroGradient' at the outlet. |
ok here is my update which i also posted in another thread :
Hey ive been following this discussion I am trying to model barrell shocks in an axisymmetric model. Inlet air is M=1. The exit is a subsonic outlet. I am using rhoSonicFoam [modified to read p , rho, T, U fields , so that the solver can accept derived BCs ] , Im using non-reflective BCs at the exit for rho, since for subsonic outlet , the eigenvalue correspding to rho is -ve. However i am not getting the inlet BCs correct . I ll summarize the Bc i have tried :-- p Inlet : totalPressure outlet : fixedValue [ static] rho inlet: fixedValue outlet : nonReflective. U inlet : 350 outlet : zeroGradient T Inlet : 250 outlet : zerogradient U & T are fine.. kindly suggest me a better combination .... |
I used the BC 'waveTransmissive' in order to have a non-reflecting BC. Find more infos here: http://www.openfoamwiki.net/index.ph...dary_condition
and here: http://www.cfd-online.com/Forums/ope...-velocity.html |
hey thank you ..
ok , they have said that the "waveTransmissive" BC is more general , but just for confirmation . can it be used for U & p [subsonic outlet ] both ??? |
Quote:
Code:
outflow |
hey thanx..
Quote:
Quote:
inlet fixed outlet zeroGradient these r my BC .are they correct ? . ill proceed with my new simulation & see where it leads me |
Well, I think your BCs are correctly defined. Let me know if your results are okay.
|
CFL criterion
I am currently simulating vortex breakdown in a conical diffuser and am doing unsteady simulations using transientSimpleFoam and LAunderGibsonRSTM model.
I have a doubt. The generally suggested criteria that CFL<1, is it the Courant Number mean value or the max courant number value??? I have a mean Courant Number of close to 0.13 and Maximum Courant Number of close to 7. (Courant Number mean: 0.130184 max: 7.10512 velocity magnitude: 3.59437) And I am able to capture the vortex. (URANS using conventional k-e and k-w models dont work!!!!) Is it the correct solution that I have got or is the solution unphysical as the CFL condition states?? Quote:
|
Quote:
Code:
Code:
Mass flux at axis = 0 |
Dear Statesman,
for my simulations (critical CD-nozzle) I'm using the 'rhoCentralFoam' solver. I read, that it should be more precise than the other incompressible solvers http://openfoamwiki.net/index.php/TestLucaG Maybe, this will help. |
I'm currently using the rhoSonicFoam solver (OpenFoam 1.6) and my Courant number is exploding as well, although I'm sure my bc are correct, since my case is very similar to the forewardStep tutorial.
Therefore I went back to the forewardStep tutorial and changed the mesh. I just moved the vertice of the obstacle corner a little right (from (0.6 0.2 z) to (1 0.2 z)). But even with this small change the courant number explodes after a while. Since the changing of the mesh causes some cells to be deformed and some getting a bit smaller I decreased the time step to 0.001 (from 0.002). But it didn't help. For me rhoSonicFoam only worked for the turorial cases. What can I do? |
sandrak, plese give some more info.
what are your BCs? what is your U? how is your start CoNum? what are your initial values? what schemes do you use? 1. rhoSonic is just stable for Ma>2. If you use a lower Ma, you need a far smaller timestep. 2. you have to use bounded schemes for div. rhoSonic solves the Euler Equations, they are convection dominated and if the convection is not bounded, the solver is unstable. |
Hi Sandrak,
maybe you should try to use 'rhoCentralFoam'. According to the literature I gave in my last post, this solvers is more accurate than 'rhoSonicFoam'. Furthermore, from my point of view it seems to be even more stable, as well, at least in my case. Generally, my problem is that pressure waves are not transmitted across the output. They are reflected, even tough, I use the 'waveTransmissive' BC for p at the outlet (I am currently testing different values for lInf, so maybe I will get better results in some time). With 'rhoSonicFoam' my simulations always crashed after the pressure wave has been reflected. With 'rhoCentralFoam' the pressure wave is reflected as well, however, the simulation does not crash. It's just that the pressure wave will travel towards the inlet of my nozzle. Thus, I suppose that 'rhoCentralFoam' is more stable. Furthermore, the shock is resolved more distinct with 'rhoCentralFoam' than with 'rhoSonicFoam'. |
Sandrack
So you are where each of us [ me , Julian , Joern] was a few months ago.. Please post your BCs that you are applying so that we can know better what you are actually doing.
Just read CFD texts to understand the above mentioned items Julian I ve been using sonicFoam with Minmod schemes for divSchemes. & backward for ddtSchemes. SO far I'm very happy in terms of both stability & results. However would you mind sharing with me the boundary conditions of rhoCentralFoam ? I used the same as i posted earlier , but my code wouldn't run. |
Thanks for the last post Mihir, you have stated the problem quite well.
Here are my boundary conditions I use for my simulation and a brief explanation of what I am doing: My domain is 2D, axi-Symmetric and consists of a CD noozle,only. That means, I do not have a far field before or after the nozzle. That's probably why I get problems with the outlet BC, because, if I had a far field, the pressure waves could leave the outlet and due to increasing cell size, the waves would be damped, so that at the farfield outlet, there would be a weak BC interaction, only. Anyway, I induce the flow with a pressure difference at dp=300mbar. At the inlet I have atmospheric pressure and thus at the outlet the low pressure. I am using rhoCentralFoam. I have uploaded a little video of the pressure contours:http://www.youtube.com/watch?v=-hhriqus2-8 The BCs are: p Code:
dimensions [1 -1 -2 0 0 0 0]; Code:
dimensions [0 1 -1 0 0 0 0]; Code:
dimensions [0 0 0 1 0 0 0]; Code:
//fluxScheme Tadmor; // KT Code:
solvers If you need more information, let me know. Mihir, could you also post your fvSchemes? I'd be very interested. Maybe also you rBC setup for P U and T. Thanks. |
Thanks for your replies, they helped. As I said, my case is very similar to the forewardStep case, just a slightly different mesh.
U: inlet fixedValue: (2 0 0), outlet: zeroGradient, wall/obstacle: fixedValue (0 0 0), top: symmetryPlane p: inlet fixedValue: 1, outlet: zeroGradient, wall/obstacle: zeroGradient, top: symmetryPlane The shock waves were a really good hint. In my case a pressure wave was reflected at the obstacle and travelled back to my inlet, where I had stated a constant pressure of 1. It happend that a region of very high pressure and very low pressure were at a small distance and thus I got very high velocity behind my inlet and that was, what caused the crash. After I changed the p bc at the inlet to zeroGradient as well, the program runs stable, even when I change the velocity at the inlet to Mach smaller than 2. So thanks. I understand the problem much more now. |
sandrak,
what you discribe is a problem of rhosonicfoam. the solver is a "direct" solver for the decoupled euler-equations. if you use Ma 2 as speed the shockwaves all point into your domain, thats ok. but the speed is not fast enough to transport reflected shockwaves. if you use Ma 3 it should work. the real problem is, that the decoupled equations produce an error in U. If the speed is fast enough the solve of the mass equation (for rho) corrects this error. if the speed is slower this error is not corrected. An solution for that gives the sonicFoam solver. This solver does an pressure-correction (PISO) to correct U and p. there you should be able to use all Ma speeds correct with a possible CoNum of ~1. (The BCs have to be set right) For sonicFoam make shure that you do outer an inner corrections (fvSolution-PISOControls). If one of them is 0 you never solve the pressure equation and do no correction. |
All times are GMT -4. The time now is 19:09. |