Hello !

I'm simulating a supersonic 30mm shell (Mach2) in the air. The residals are converging, but no more than 5e-3...

Is it important ? can I trust this result ?

And what are exactly the residuals ? (I understand them as the difference beetween 2 cells... Am I wrong ??)

Thank you very much !!

Cyril

Residuals are the differences in the value of a quantity (for example x-velocity or y velocity or k,ecc.) between two iterations. This means that the more the residual is low the less the results will change if you will continue to iterate. Residuals depend from the models that you use (for example with natural convention normally they don't decrease a lot because there isn't a strong fluid dynamics component) and from the initialization because if you use an initialization that is very close to the final solution residuals will not decrease a lot as you use an initailisation that is far from the final solution. Often you can find a period during which residuals seem not to decrease but if you continue to iterate they restart to decrease. Furthermore residuals means mathematical convergence; you have to monitorate a quantity that is fundamental for your case (for example the lift or the drag, ecc.) and you have to decide if your case is converged to look both (often to the residuals and to the fundamental quantity (if your fundamental quantity doesn't change even if you continue to iterate your solution will not change more). I hope this helps Regards Emanuele

Hi,

I agree with Emanuele's answer, what you can do to decrease the residuals is to do the calculation in double precision (2ddp for 2D case and 3ddp for 3D case).

The problem, with double precision, will be the time. I'm working with some hudge meshes (about 3-4 1.e6 cells !)

Here is what I've got : http://img105.imageshack.us/img105/8...nstitre2xk.png.

My geometry fits the shockwave. Here is what I study... http://img149.imageshack.us/img149/6...nstitre2xv.png

What do you think...?

Hi,

First of all 3-4 e6 cells, it's really really heavy!! Can't you input a mesh which corsens when you move out from your object of study (use size function for this). You will decrease the number of node elements and therefore earn a lot of time for the calculation.

Furthermore, for shockwave study, you need at least a second order discretization of the pressure and velocity, the first order will give you wrong results.

Check in the Fluent manual if you can't increase the convergence speed with another coupling between pressure and velocity (SIMPLE, SIMPLEC, PISO).

I hope it will help you.

[MrNavierStokes]

I know this thread is 10 years old, but thinking about how much I struggled in the beginning learning CFD only because of false information being spread and that students could read this I'll answer it.
The Residuals are NOT the difference in the value of a quantity between two iterations! Judging the convergence behavior of a simulation based on this would be a poor approach.
Since the governing equations (NS, continuity etc.) describe the conservation of fundamental fluid-quantities and the discretization method is the Finite Volume Method, the residuals are a measure for the imbalance of a fluid-quantity in a finite volume (flow of quantity out of FV - flow of quantity into FV = R). So if we look at the continuity equation for example, the residuals give us a feeling for the mass getting lost or being produced inside our discretized flow domain. The RMS values in CFX are mean values (Root Mean Square) over all finite volumes.

Regards,
Alex.

[wilandlane]

Alex,
Thanks for your post. You're right, mis-information can cause lots of problems, so it can be very helpful when you provide any helpful information you can. Your answer is spot and and should prevent confusion for at least a few people.

[sidaero]

Hi this siddharth. My problem is regrading moist air flow condensation on airfoil in transonic flow. Velocity=258 m/s (M=0.8) Temperature=259 and Pressure=65600 Pa
I am working Komega model with a Y+=2
The continuity residual does not converge when i perform the analysis in pressure based solver- coupled solver.. I am getting divergence and sometimes the continuity residual gets stuck near some place and does not converge.. My mesh aspect ratio is 740 and the transition is also smooth. But still the solution is not converging..
I even tried by putting first order scheme for few iterations and second order later and it also did not work..
can anyone give some suggestions about to how to proceed with this???
Thanks in advance..