Guys, Sometimes after initializing the problem in Fluent and triggering the calculate button, a residual/residuals start from a big non-zero magnitude. For instance, to me, it in many cases happens for some convection-diffusion equation when I'm simulating combustion. Interesting point is that the results looks ok and have good agreement with experimental results. In this page:
http://www.afs.enea.it/project/neptunius/docs/fluent/html/ug/node833.htm
It's said that:
"For most problems, the default convergence criterion in ANSYS FLUENT is sufficient. This criterion requires that the scaled residuals defined by Equation 26.13-4 or 26.13-9 decrease to 10-3 for all equations except the energy and P-1 equations, for which the criterion is 10-6."
As it is said, the residuals need DECREASE TO 10-3. Then it means that it doesn't matter from where the residual starts, it should finally decrease to 10-3.
Another question:
3. Why does it happans? (I mean why does the residual start from a non-zero magnitude?) and How to figure it out?
I've attached two screenshots of the residual of a project for instance.
In my honest opinion there are many situations where this statement from the ANSYS Fluent manual is rather misleading, if not even wrong. In particular in CFD simulations with strong heat and mass transfer almost the entire physics, material parameters and thermodynamics is bound to a very good convergence of the energy equation. In my opinion a scaled residual (RMS Res) of 10^-3 for the energy equation usually leads to rather physically wrong fluid temperatures (i.e. large errors in comparison to the real physics) with the corresponding consequences for the accuracy of the overall simulation.
The CFD best practice is:
1) define meaningful, local and sensitive physical target quantities (e.g. a temperature profile or a distribution of a certain sensitive species of your mixture).
2) run a series of CFD simulations on a reasonable resolved mesh (not the coarsest one) with systematically refined (and reached !!) convergence criterion, i.e. RMS Res
Be careful about the term " scaled residuals " ... The guess iteration can be far from the solution and the residuals appear having high magnitude. But the second figure does not show a convergent trend
In my honest opinion there are many situations where this statement from the ANSYS Fluent manual is rather misleading, if not even wrong. In particular in CFD simulations with strong heat and mass transfer almost the entire physics, material parameters and thermodynamics is bound to a very good convergence of the energy equation. In my opinion a scaled residual (RMS Res) of 10^-3 for the energy equation usually leads to rather physically wrong fluid temperatures (i.e. large errors in comparison to the real physics) with the corresponding consequences for the accuracy of the overall simulation.
The CFD best practice is:
1) define meaningful, local and sensitive physical target quantities (e.g. a temperature profile or a distribution of a certain sensitive species of your mixture).
2) run a series of CFD simulations on a reasonable resolved mesh (not the coarsest one) with systematically refined (and reached !!) convergence criterion, i.e. RMS Res
Filippo Maria Denaro Thank you for reply. Could you please add more details on the points you mentioned in your reply?
But both the calculations looks ok.
There were already good answers. But to answer your questions: the residuals are usually positive and non-zero. Especially at the beginning of each iteration cycle, they can have large values. That doesn't matter, as long as the residuals significantly decrease and reach a relative or absolute convergence criterion. Besides, scaled residuals can have an even larger or lower magnitude. But as Dr. Frank said, residuals are not everything and you should have a look at the convergence of your targeted quantities.
From your example residuals alone it is hard to see convergence. In the first one, the h2o fraction residual is quite high. In the second one, the residuals are gradually increasing, which is not favourable. These are transient simulations, right?
Julian Vogel Thank you for great answer!
But for each time-step the residuals have fallen, properly and the result looks ok (after checking out the contours of pressure, velocity, etc). Yes, there is a transient area/point in my domain for deflegration to detonation. Might I ask you how did you know it?
Yes, but the residual for the h2o fraction is really high, around 100 in the first and 1000 in the second figure. If this is a fraction value somewhere between 0 and 1, this probably means that the result is not a good approximation of your equation system. But it depends on the magnitudes of the variable and the residual scaling, so it's hard to give advice without further knowledge.
If it was a steady simulation, the residuals would be quite oscillatory. In a transient simulation the oscillations would just be due to the time steps.
I’ll add my teo cents. The residual is not a physical quantity but a numerical, and it provides information about how close your governing equation (discretized) is balanced. In other words, all terms make a total contribution and if that residual is high it means that one or more are leading to unbalances at the control volume. Since that is a numerical value it will not ever be zero as we are always told in our PDE classes.
An interesting way to see this, is to initialize your solution from a converged solution erasing the history. You will see that your residual will be a flat line and you can think “my solution is stalled”. If you start with a good guess the solution will be similar. If your IC is far from the final solution then you will see a huge drop.
- Badges
- Science topic