Hi all,

Okay, it sounds a strange question. Of course RMS Res is better if smaller. But I have a question about my ploblem.

The image bellow is the convengerce history of a simulation of mine (steam in the main drum of a industrial boiler).

After around 200iteractions the RMS Res value reaches its minimum. After that, the value rises again and even after more than 2000 iterations, the low level of this first valley is not reached anymore. (turbulence Res follows the same trend).

Normally I would expect a value of RMS REs decreasing (with noise, of course) till a certain level and than resting there. Not rising again and resting on a higher level.

What is going on? is my simulation not converged? and where should I stop it and get the results? around 200 iterations with the minimum of RSM Res or after 2000 iterations, with high Res but probably closer to a fully converged result?

Thanks in advance

Anderson



ZOOM:

Are you trying to get the system to converge or are you ok with it bouncing around like that and just want to know which RMS Res will get you close?

If the data you want is simple (Pressure Temperature Velcoity etc.) you might want to create a "watch" that follows the values as the problem iterates. For example, my pressures actually stabilize about 20 iterations out for my model even though the problem won't converge for another 10-20 iterations. That would tell you whether or not the data you want is fairly stable.

I have a model whose Res look exactly like this. I was able to get it to converge by playing with the blend factors.

-W

Hi,

This question has been asked many times. Search the forum and you should get lots of hits. It is also discussed in the CFX documentation

In short: 1) It is usually caused by some small instability which is causing the flow to fluctuate. This fluctuation could be real (eg vortex shedding) or a numerical artefact. 2) Plot the important parameters for the flow. It might be heat transfer to the tubes in a boiler for instance. If this parameter is not fluctuating then your answer is probably OK as it is and it is not worth bothering to get better convergence as it won't change the answer anyway. 3) If you do need to gain better convergence, try: a) Increasing the physical timescale b) Switching to local time scale factor (but switch back to physical timescale for final convergence) c) Switching to a transient model and marching it out in time to steady state.

I general don't like adjusting the blend factors below 0.8 or so. If you adjust the blend factor below this to get convergence introduces a lot of first order discretisation which will make your simulation inaccurate.

Glenn Horrocks

Thanks Wooster and Thanks Glenn Horrocks

I will give it a try with the blend factors and with the local time scale (Ive already played with the physical timescale)

If I get any news, I will keep you posted.

Cheers

Anderson

Hi Anderson,

I would also check the volume ratio's in your grid. If you have a very sudden change in element size in a region of high gradients, such as at the edge of the inlfation layer between the last prism and first tet, the solution will oscillate. The situation I described is most common in unstructured meshes. If it is a hex mesh, the problem is often due to striping. Fixing these can make a HUGE difference in convergence.

-CycLone

Hi Anderson,

Residuals tell you how well the equations have been solved but small values of residuals don't tell the whole story. As you mentioned yourself, you expect the residuals to continue decreasing and this is certainly the desired behavior. When you see convergence as you have here, it indicates a problem. Given that the original convergence was good, I would guess that there may be some separation that has occurred somewhere in your model. If this is the case, it may not be possible to get a steady state solution, because the shear layer cannot be adequately damped by the turbulence model. Increasing the timestep can sometimes help subdue transient behavior. If the problem is numerical instability, decreasing the timestep may help. Running with double precision on can also help if the grid quality is poor.

I would first suggest writing the residuals to a results or backup file to determine where the fluctuations are occurring. In some cases if the quantities of interest are stable and the the solution is fluctuating in a region which is not of great consequence to your solution, you may be able to safely ignore it. If this is not the case, you may need to take action.

If the mesh quality is poor in the same region, consider fixing it. If that is not the case and the solution is showing transient behavior, you can consider running a transient simulation instead and calculating the transient average values of velocity, pressure, temperature, etc. This is generally a better approach than running for several thousand iterations trying to converge a solution that does not have a steady solution. The run time will probably be a bit shorter in the end and the average solution will be more appropriate. As a bonus, while the transient analysis would not require you to write transient results along the way, doing so also allows you to make some pretty cool animations!

-CycLone

Good point that I failed to make, Glenn.

If you do play with blend factors, the CFX manual says 0.75 is the lowest you should go. However, the lower the factor the more the answer turns into a first order approximation and thus you can be off a good answer by a lot. If you decide to change the number, start high (0.99) and work your way down.

-W

Hallo,

Thanks for all the good explanations. You all helped a lot!

I already know that I need a finer mesh, but I have a small computer limitation (I am working on getting a new one).

Moreover, I realised that the higher values of residuals are near the outlet of the drumm (region where the steam is "sucked out" the equipment). Luckly this region is not so important for me.

I will play a bit with the parameters you suggested and also try the transient analysis (with its animation ). If anything else comes up, I will let you know.

Thanks again and have fun with your simulations

Anderson

Just to Register:

Found a way! It was the transient thing. It seems that the turbulence is so high near the outlet that it disturbes all th e flow in the drum and a transient aproach is needed to see it. After playing a bit with the transient parameter I got a RMS Courant around 5 and my residuals are smaller than 10e-5.

Really good

Thanks a lot to all of you!

Not to burst your bubble, but be aware that residuals mean a different thing for Steady and Transient runs. The transient residual indicates that the timestep is converged, which includes the transient term. In a steady analysis, the transient term is not included in the residual because a steady state is desired.

-CycLone

hmmm didn´t get this one.

So maybe the transient terms are damping a bad result? :-/

Okay, I am aware that I still need a finer mesh, but I really though that RMS residuals between 10-5 and 10-6 were quite good, even for transient analysis. Moreover, now I think that this is really a better way to deal with my case, since I have some deadzones, where slow velocities and unstable eddys are present. I don´t think these zones will ever reach a steady condition.

yeap, you have just bursted my bubble, but thanks a lot for awaring me of this!