Dear Friends,

In my simulation(using CFX), convergence history plots are wave line.

I didn't know the problem.

Please hele me. Thank you in advance

Eric

Hi... I think there's some discussion in the help manual about the bouncy behaviour in solution convergence. It could be due to the transient effect in the flow and many other reasons. Are you using SST model? Try putting more details about your problem.

Thank you for your kind reply.

I simulate the distribution of compressible air in an cylinder. Steady.

Maybe the quality of the mesh is poor. I just use CFX-mesh to generate the mesh.

Hi Eric,

Try increasing your timestep by a factor of 10. If you used the Auto Timestep, look at your out file to see what the solver came up with.

Regards, Robin

Mr. Robin, Thank you. As you said, I used Auto Timestep. How can I choose a correct timestep? THank you very much.

As Robin said, you can get the Auto Timestep in the result file, then determine the timestep you want to define in the definition file or result file by editing them. For steady flow, theoratically, the timestep is a dummy marching.

But I did not get why Robin suggested to increase the timestep. Usually it should be reduced for better convergence, right?

Regards,

Thank you very much. I will adjust the setting. Many thanks

Hi Bian,

This is common misconception. It depends on what is happening. If the numerics are unstable, it can help to reduce the timestep and thereby relax the equations. However, this will usually manifest itself as sharply varying residuals.

What Eric described was a sine wave, which indicates a transient variation. If this is the case, reducing the timestep won't help because you will resolve the transient fluctuation to an even greater degree. By increaing the timestep, you can often get rid of these fluctuations.

The solver will tolerate very large physical timescales. In my experience, the auto timescale is usually too small. It uses a fairly conservative estimate for the timescale that is sufficient to keep the solver stable (i.e. it is not likely to overflow) but may not be optimum for convergence. I usually increase it by a factor of 10, especially early in the run when you have a lot of transients from the initial guess.

In many cases, a good estimate for the timescale is to load a backup or results file into Post and compute streamlines, then look at the maximum or lenght averaged value of time on the streamlines (the maximum value can be very large if some streamlines get caught up in a recirculation zone) and use this for your timestep.

Eric: to change the timestep, go back to Pre and change from Auto Timescale to Physical Timescale, then input your value. You can also change this using the def file editor or on the fly, but you will have to make sure you delete the length scale option and add in the Physical Timescale parameter. At version 11.0 there is a multiplier for the auto timescale, which is very convenient.

Regards, Robin

Dear Mr. Robin,

Thank you very much for your explain.

Now, I changed the Auto to Physical timestep, and the plot is very beaufiful.

Mang thanks

Best Regards

Eric

Hi, Robin,

Since CFX is a fully coupled and implicit solver, there are a lot of things I did not have experience on. I knew the way to determine timestep by using streamline, but never did that. Overall, if the residual plot is like damped sine curve, it can be improved by increasing timestep. It seems doing this can reduce the simulation time for convergence as well, isn't it?

Thanks,

BB

Hi Bian,

You are correct. A larger timestep will reduce the number of iterations, but at the risk of instability. As a rule, I would recommend always starting with as big a timestep as you can get away with.

In 11.0 you can specify a multiplier on the AutoTimescale. When I have run dev versions of 11, I nearly always set this to 10x.

Regards, Robin

This approach seems to "artificially" damp out the bouncy behaviour in the solution residuals. It's still useful to check if the transient effect will affect your steady-state results. Even if you get a smooth residual plot, it doesn't mean that your solution will be more accurate than before.

Hi TB,

The timestep only affects the rate of convergence.

There is nothing "artifial" about this. When you run the solver in steady state mode, the transient term is only used to stabilize the equations. At convergence, the transient term goes to zero and it doesn't matter how big or small your timestep is.

If there is a transient effect that needs to be considered, you should run a transient solution. Although the behavior of steady state convergence may look like transient behavior, you must keep in mind that the solver is not actually solving an accurate transient.

Regards, Robin

What I want to say is when bouncy behaviour occurs in your residual plot, it may indicate that the flow is unsteady, and it's sometimes worth examined and should not be overlooked. Some flow problems are highly unsteady, even if the constant boundary condition is applied. Of course you can use Robin's approach if you are sure that transient effect is not a problem.

Hi TB,

That is a very general statement to make. I would hazard to classify any case that has bouncy convergence as transient. There are many reasons why this can occur in a steady state solution, timestep selection only being one of them.

If you cannot get the solution to converge at any timestep and you have eliminated any possible grid problems (large volume ratio's, particularly at the edge of inflation layers into the tets can often lead to instability), then you might conclude this. But if a steady state solution is acheivable, there is no need to assume the flow is transient because of it's convergence history.

Regards, Robin

Oh yes. That's exactly what I do for one of my flow problem. I just want to point out that not all bouncy behaviour is due to the timestep size.