fluent 经典问题 Fluent 收敛判断和 solver选择

Fluent

收敛判断和

solver

选择

从

上转过来 的，虽然是英语，但是静下心来慢慢读一读能学到很多

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

Sysnoise's Users_Manual

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

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