[转帖] 关于收敛

carboy2199

[Fluent] 收敛判断和 solver选择
问题 ：----------------------------
Hi! I have tried an external aerodynamic problem in Flunet. In it, I want to know pressure distribution over the wing assembly.
I have used Coupled-Implicit-Spalart Allamaras solver with courant number 1 initially. I gave pressure-far-field BC in elliptical boundary around wing assembly which is 10 times larger.
After 5000 iterations also, my solution is not converging or continuity and momentum residuals are not coming below 1e-3. They oscillating between 1e-2 and 1e-3. Viscous residual is less than 1e-3.
I have changed under relaxation factors, discretization schemes also. Still, I am not able to achieve residual lesser than 1e-4.
I want any one users help. I am conveying my advance thanks ..........
with regards, vengi.
  
某人的回答
There';s a few things that could be going on.
One possible answer is that your model is converged (that';s always the happiest answer, isn';t it?). The residuals you are looking at are normalized based on the residuals of the first iteration. So if your initial guess is pretty accurate, then your first residuals will be small, and all of your following residuals will be small as well, but since they are normalized according to that first small value, they look large. This typically shows up in the continuity and momentum residuals, and sometimes even in the x, y, and z velocity residuals (at least in the coupled solver). One thing you should be doing with your model is monitoring other factors besides your residuals. If you';re looking for the pressure distribution, then define a few points along your airfoil and monitor the pressure at these points. You should also monitor at least the lift of your airfoil. You can find these monitors under solve->monitors. Judge convergence by when these have leveled off. While your model is solving, you will probably have to go in and clear the data in the monitors or adjust the scale of the axis to get a better idea of when they';ve truly leveled off. That can all be done in the windows where you defined the monitors.
Another possibility is that your model isn';t converged (the less happy of the answers). If that';s the case, then there';s lots of possible reasons. One common one is the use of the Coupled Solver in low speed flows. Since the coupled solver is a density based solver, it can get hung up in incompressible flow regimes. Typically, I only use the coupled solver for flows over Mach 0.7, but I';ve used the segregated solver from Mach 0.05 up to Mach 1.2 (paying CAREFUL attention to the mesh where shocks form). Another possible problem is that its an unsteady problem. If you';ve stalled, you could be shedding vortices at some frequency. The SA turb model does alright with small separation regions, but a large separation region (say behind a shock at some angle of attack) can cause it to fall apart. It was originally designed for 2D airfoils without any separation. They';ve modified it some to try and make it work in 3D, and to try and help it handle separation, but I still haven';t had much luck with it. There could also be some issues with your mesh. Pay attention to your y+ values and the rules concerning them.
Either way, you really should be monitoring more than the residuals to judge convergence. I';ve seen it a lot here, where someone will call a model converged because the residuals dropped below 1e-03, but when I';ve taken the model and continued with the iterations, I';ve seen a dramatic change in the forces. I';ve also seen it where someone will be 8 or 9 thousand iterations in trying to get the residuals to drop, but the forces have been steady.
Hope this helps, and good luck,
Jason
又有一个人来提问
Hi Jason, could you tell me more about using the segregated for transonic on ligthly supersonic flows? I tried it with the AGARD 445.6 wing for flutter determination and I had very good results for transonic flows. So, If we take care of under-relaxation factors and we make a good mesh, can segregated solver be used even for transonic flows?
luca
接着回答
    You can use the segregated solver for transonic flows. It tends to diffuse the shocks compared to the coupled solver, but you can fix that by using a refined mesh. A lot of times that';s what I have to do here, because I';m running into memory limits, and increasing the mesh by 10-20% still fits in the available memory, where switching to coupled solver doesn';t (coupled solver uses 1.5x to 2x the memory because it stores the solution to the last iteration).
    As far as solver settings... it';s very important to set your control limits. For temp and pressure, I calculate the delta between freestream and stagnation, and I double that. If I have a problem getting the model to converge, I may cut that down to about 1.5 to 1.2 times the difference between freestream and stagnation. (So my Pressure limits are Pstatic + 2*Q and Pstatic - 2*Q) I set the pressure and momentum URFs to 0.5 and 0.4, leaving energy at 1. The SIMPLE Pressure-Velocity coupling tends to work well... I';ve gotten some recommendations on switching to PISO, so I';m actually trying that right now. I tend to run for 10 to 50 iterations with all the default discretizations and the turb eq turned off. Then I turn the turb eq back on (I don';t go all the way to convergence like some people recommend... I haven';t found any benefit... I usually only do about 50 iterations with these settings). After that, I set everything to 2nd order discretization and run to convergence. These settings have worked well for me on aerodynamic models with little or no separation, and they';ve worked (with a little playing around in the URFs) all the way to Mach 1.2.
    I have run bluff bodies at subsonic compressible to transonic speeds (typically a symmetrical model to get more of a "time averaged" solution... this avoids the oscillating vortices and cuts out the need for the unsteady solver... I haven';t run transonic of a full bluff body, but I have run Mach 0.5ish with a full model and the unsteady solver... that was a while ago though, and I don';t remember if I had made any changes to my solver settings). The coupled solver is a poor solver for this kind of model because of the large separation region aft of the body. This becomes a difficult model for the segregated solver as well, but I';ve had good luck running it with default discretization and the turb model turned off for about 100 to 200 iterations... then turning on the turb model, and lowering the energy URF to about 0.7 and running for another 100 or so iterations. Then upping the energy URF back to 1 for another 50 or so, and then switching to second order and running to convergence.
    The most important things I have found are paying attention to your mesh (or using adaption or dynamic adaption to resolve shocks... you don';t need to refine them all the way for overall forces, but you might for flutter analysis) and setting your control limits.
    Hope this helps, and good luck,
    Jason
Thank you Jason, your explanations are complete and well detailed as usual. I run the Agard 445.6 at mach 1.141 and had no problem with convergence. I just set momentum URF to 0.4. Yes you';re rigth when you say coupled solver requires more memory. In fact if I use the segregated I can make a more refined grid because it requires less memory. This is great! SIMPLE scheme seems to work well and I didn';t need to switch to PISO...and I had no problem to solve the flow with transonic or supersonic flow. Thank you again for your answer. I just needed to have a confirm somebody else tried to use the segregated solver for not subsonic external flows. Luca