Hi,

Can anyone please explain the significance of relaxation factors and their exact function. I just know that reducing the under- relaxation factors helps speed up the simulation. But how exactly does this happen and what goes on when these values are reduced? How do we know which values need to be reduced and when (e.g., pressure, momentum, turbulence etc)?

My transient simulation is runing with a time step size of 2*10e-5 and 200,000 time steps. I'm also using the Adaptive time stepping method. But the simulation is extremely slow and looks like it'll take months to complete the simulation.

Does anyone have any suggetsions? There are 124,000 nodes in my geometry. The time period is 2 sec and I want to run the simulation for 2 whole cycles. Any attempt at increasing the time step size resulted in errors.

Thanks, Vidya

Hi Vidya,

They may be different approaches but as a brief description you can take a look at here. Relaxation factors: When you get the answers in new iteration (after solving the matrices) the relaxation factors determine your new parameters. In fact the new parameters are defined as the old parameters plus a factor (less than 1) times the difference between new and old parameters.

New= Old + (relaxation)* (New- Old).

It helps convergence. It is very important to choose proper relaxation factors for your problem. There are some rough rules for some cases. For example you may use a relaxation for momentum and 1 minus that relaxation for pressure eqn.

For more information take a look at CFD books.

Mohammad

Thanks Mohammad.

In your case if you want to increase the time step size, I would do the following,

1. Do not disturb the default URFs. (leave them alone they are fine).

2. I would increase the post AMG sweeps in AMG settings to get better convergence for each level, I would make them 3 from 1. (If I am doubling the step size).

Or find out the most difficult variable to converge, in most cases its is pressure, which is fixed AMG cycle (V cycle), I would increase its post AMG sweeps to 3 and keep the flexibale Cycles post sweeps to 1 as default. (Yes if the most difficult var to converge is not pressure, set its AMG cycle to V and increase the post sweeps).

I guess with these you can at least double the step size. Try it.

Hi Zxaar,

Can you elaborate more on what you just said....... how do I change the AMG solver settings? And what impact does this have on the solution?

by changing the step size , the change in solution also increases, so this means that I will have more deltaPhi change with timestep = 1E-03 than with 1E-05. So if you try to use large time step, and the solution at each step is not converged significantly you will introduce errors. This might lead to unstablity in solution.

What AMG should do is make you acheive tighter convergence at each time step. By incresing post AMG sweep, you force more convergence at each time level, enaling you to switch to larger time steps.

Now , what i said was , chose the variables for which you think it is difficult to get convergence, pressure is one of them. So for them chose fixed cycle and increase the post sweeps, so you force convegrence on it. Keep other variable sweeps same, so that the computational effort does nto increase very much.

You can find multigrid controls at menu

Solve->Control-> Multigrids.

Hi,

I made some changes as you suggested, but I still don't get the real idealogy behind doing all this. I couldn't make sense of what was said in the Fluent Manual either.

Can you please elaborate on what you're trying to explain?

Thanks a lot.

Vidya

I know it would be little difficult to grasp what I said, let me try again. (for more details try finding out multigrid methods).

Usually the variables are solved in the manner: A.X = Src Wher {A,X,Src} are matrices. X represents the variable under consideration, for laminar case it is { U,V,W,P}. So for each iteration, you update X = Src . A^-1 But the problem with this kind of solution method is it could give poor convergence if the meshes are very large or too fine. One cure for this problem is to use Multigrid Method. As names suggests there are multigrids involved in this method. Now the questions is , if you provided only one mesh or grid, what are these other grids those are involved. To understand other girds, imagine that you fuse few cells to make a bigger cell. You can have another grid now. You can further fuse these fused cells to make even coarse grid. And so on. So now you have : 0 level grid : you provided. 1 level grid: made by fusing cells from zero level. 2 level grid: by fusing 1 level cells so on ...

What role these grids play, well what we do is once we have a solution at 0 level, and since the equations do not converge here (0 level) you have some residuals here. We tranfer these residuals or solution from 0 to 1 level grid, and solve them there, and then we move to 2 level so on. Once we have solution at last level, we transfer back the correction from n level to (n-1) level. And run some iterations at (n-1) level, again transfer corrections to n-2 level and so on. Till you reach, 0 level or your main grid. Here again you perform some iterations.

These iterations that you perform after getting correction from higher level grid, is post AMG sweep . The iterations you perform before tranfering solution to higher level are pre AMG sweeps. by default they are 0, and its better to be zero, so do not change them.

Now whats happening in you case is when the soltuion shifts from one time step to another, if you do not have good convergence at that level, you introduce errors. Those could lead to problems. So what we do is change the post AMG iterations to force more convergence. Best part is AMG is in two forms one FIXED cycle and another flexible cycle. So put allthe troublesome vars in fixed cycle and increase its post AMG sweeps, So that the computation effort does not increase very much, but you can now have better convergence. This is what I suggested, hope this make sense.