CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   Residual rise (http://www.cfd-online.com/Forums/fluent/78401-residual-rise.html)

 Mohsin July 21, 2010 04:08

Residual rise

hello

I hope you people are doing well. During my fluent's simulation using k-Epsilon model the residual level reduces (trys to converge) but at some point in the calculation the residauls for k and epsilon starts to diverge but as I have set a lower level for the residuals of K and epsilon. I still get a converged solution.

1. My question is that if the residuals for K and epsilon or any parameter show a diverging trend and the solution gets converged. Is it acceptable?or the residuals are always supposed to show a converging trend? (If we only observe residuals for convergence criteria).

2. My second question is that As the residuals for K and epsilon showed a diverging trend, I kept their convergence criteria to 0.005 each. Is this an acceptable limit?

Thank you.

Mohsin
South Korea

 Chris D July 21, 2010 09:21

Quote:
 Originally Posted by Mohsin (Post 268276) ...as I have set a lower level for the residuals of K and epsilon. I still get a converged solution.
What do you mean by this? You can't really tell if a solution is converged just by looking at the residuals.

 kdrbrk July 21, 2010 10:02

As far as I know, to say that a solution is converged, forces should stay the same. So you should better monitor force coefficients. When the coefficients stop changing, than your solution is converged.
This happens to me between 10e-5 and 10e-6.

 Chris D July 21, 2010 12:01

I think it depends on what you're actually looking for. For flow over an airfoil, monitoring forces would be good. If you're solving a heat transfer problem, though, you might want to look at surface temperature.

 -mAx- July 22, 2010 01:27

Monitoring or not (I would recommend,cf: http://www.cfd-online.com/Forums/flu...ns-querry.html), you have a problem with turbulence equations.
The residuals are rising or do you just get peaks?.
If they are always rising, then your calculations are going to diverge.
*maybe you have a poor turbulence initialization
*it can also be caused by poor mesh quality

 Mohsin July 22, 2010 11:08

1. Max: I am using KE model. The residuals for K and Epsilon converge until 300 iterations but after that it doesn't converge and keep on diverging. To make their divergence slow I reduced under relaxation factors for K and E to 0.5 and the residual convergence criteria to 10^-3. so that in the mean while other residuals( which are converging) should meet their convergence criteria. By doing this i get a converged solution (based on residuals) at 1500th iteration.
The convergence criteria i used was residuals, mass flux and Surface integrals for inlets and outlets. (Cf: as (Max) suggested earlier http://www.cfd-online.com/Forums/fluent/78147-iterations-querry.html)
and I got the flat lines.

2. I always get flat lines even at 600th iteration and Mass flux is always less than 2 percent (as suggested by the Fluent manual). But residual criteria is not achieved until 600th iteration. So for convergence of the solution I should look at the three criterias simultaneuosly? Right?

3. For 1 case I ran 2 simulations (to check teh validity of the results) and both of them gave me converged solution at 1500th iteration with all the convergence criterias satisfied (The residuals, surface integrals and mass flux). I only changed under relaxation factor (for K 0.55 to 0.5, for epsilon 0.55 to 0.5 and for pressure 0.35 to 0.4) keeping all other things same BUT i got very much different results for both the simulations. ( For simulation 1 i was getting standard deviation of 1.5 and for simulation 2 i was getting standard deviation of 4.5). Does changing under relaxation factors influence result? thats what made me confused.

Mohsin
South korea.

 Chris D July 22, 2010 13:45

By lowering the under relaxation factors, you prevent solution variables from changing too much from one iteration to the next. This in turn reduces the residuals. So, what you're doing is actually tricking yourself into thinking you have a converged solution, but you really don't.

Have you tried just letting it run without changing the urf to see what happens? What might happen is that the residuals decrease initially, rise to some maximum (without blowing out the solution) and then decrease until convergence is reached.

 -mAx- July 23, 2010 01:06

I wouldn't modifiy any URF values.
Try first to fix your divergence issue.
Do a checkMesh, and check your turbulent BC

 Mohsin July 23, 2010 03:07

Chris: without Urf change I still get a diverged trend for K and E. Initially the trend was converging until around 600 iterations then it diverged to a maximum level and then remained constant (neither decreasing or increasing with a 10^-2 residual level).

Max: Mesh size is 0.21 million cells. For mesh check, The geometry has a worst elemnt with a equi size skew of 0.89 and equi angle skew of 0.79. 90 % of the geometry consists of hexahedral meshing scheme and 10% consists of tetrahedral meshing scheme.

For Turbulent boundary condition i used the formula given in the User guide (the formula is based solely on reynolds number, which lies in turbulent state) and got 4.5 % of turbulent intensity at the inlet and 4 % at the outlet. For initialization, i did simulation 3 times with three different initial values. But I always got diverged solution. probably there is some other way which can converge the K and epsilon reisduals. Can u please tell me what can be the best inittialization or any other procedure for doing this. I cant use FMG initilization because I am working in a multiphase flow regime(DPM model).

Thank you

 -mAx- July 23, 2010 04:11

Quote:
 Originally Posted by Mohsin (Post 268637) because I am working in a multiphase flow regime(DPM model). Thank you
Ok that's kind of info you should give in your first thread... ;)
Disable DPM and multiphase models and re-compute (it should be a basic flowfield).
If you don't get any trouble, then your issue could be linked to the set-up of DPM-multiphase model.

 Mohsin July 23, 2010 12:43

Max I did what you said. I did simulation without DPM but I got exactly the same results (the K and E are diverging). That means the problem is not with multiphase modeling. The problem is with flow field's turbulence modeling. What do u sugget now

 -mAx- July 23, 2010 14:21

Continue working without DPM untill you solve the problem.
*Does your Re match turbulent domain?
*Are you computing uncompressible?
*Try to compute your model on a finer grid

 Mohsin July 26, 2010 04:11

Quote:
 Originally Posted by -mAx- (Post 268738) Continue working without DPM untill you solve the problem. *Does your Re match turbulent domain? *Are you computing uncompressible? *Try to compute your model on a finer grid
The Re number at the inlets is around 30,000 to 50,000 (which should be above 4000 for turbulence as Nitrogen gas is used in a cylinder).

As gas is used so it is compressible.

At first i used 0.21 million cell grid then as you said to refine the grid so i increased the cell number from 0.21 million to 0.31 million cells. But same problem occured for K and Epsilon (After converging to a minimum point (5*10^-4) they diverged and continued to diverge until residual 8*10^-3 and then got flat).

I also checked for Near wall treatement and different K epsilon models such as Standard rng, realizable but They residual for K and epsion shows the same behaviour or doesnt go below 10^-3 residual.

Any other suggestion? or whateevr i m doing is fine?.....

 -mAx- July 26, 2010 05:10

*Are energy equations turned off or on? (check your Mach Number for compressible or uncompressible flowfield)
*You can also try switching to double precision solver
*Also try to switch on 2nd order scheme for K and E
*Regarding the finer grid, are you not able to handle a 1 million cells mesh?
*Can you display pressure distribution and also velocity before divergence occures, and while it diverges
*Display also the residuals

 Mohsin July 27, 2010 04:04

Quote:
 Originally Posted by -mAx- (Post 268864) *Are energy equations turned off or on? (check your Mach Number for compressible or uncompressible flowfield) *You can also try switching to double precision solver *Also try to switch on 2nd order scheme for K and E *Regarding the finer grid, are you not able to handle a 1 million cells mesh? *Can you display pressure distribution and also velocity before divergence occures, and while it diverges *Display also the residuals
*The energy Equations are turned off. Mach Number lies in subsonic region as the velocity of the gas is only 15 m/s.
*The scheme is already second order. and for pressure I am using PRESTO scheme because it is suitable for swirl flow.
*For finer grid (upto 1 million cells) i dont have such a powerful computer( I have Intel Core Quad with 4 cores ) I can arrange another one in a day or 2 and merge them to run simulation wih 1 million cells and come back here and let you know.
*I didn't understand you last 2 points. Display pressure distribution, Velocity and residuals before and after divergence. Could you please elaborate on that?

The model is a verticle cylinder with 5 inlets and 3 outlets. 1 inlet is at the top from where particle plus gas enters and 4 other inlets are at the middle sides from where gas enters which provides swirl motion to the particles which eventually moves out from the three outlets. I m using KE Realizable model with non equilibrium wall functions. Solver is Pressure bases, 3d, Steady. For particles DPM modeling is used.

Thank you very much.

Mohsin

 -mAx- July 27, 2010 05:27

post picture of pressure on a middle plane (prior and after divergence), also a picture of velocity(prior and after divergence)
Also a picture of the residuals.
Is your geometry scaled? (gambit doesn't give any unity, if you don't specify any in fluent, the your geometry is based on meter, ie 1 == 1m)

 Mohsin July 29, 2010 02:36

5 Attachment(s)
Quote:
 Originally Posted by -mAx- (Post 269021) post picture of pressure on a middle plane (prior and after divergence), also a picture of velocity(prior and after divergence) Also a picture of the residuals. Is your geometry scaled? (gambit doesn't give any unity, if you don't specify any in fluent, the your geometry is based on meter, ie 1 == 1m)
Thank you Max.

My geometry is scaled. When i started Fluent I changed all the dimensions into mm and then scaled them. (But when i click on summary it gives all values in meters).

I have attached 5 pictures as you asked for.

1. Residuals after convergence. (the residuals converged after 1200 iterations but after 550 iterations K and epsioln's trend was diverging). Although all the residuals were converging.

2 and 3.Contours of static pressure and velocity after convergence at 1200 iterations.

4 and 5. Contours of static pressure and velocity before divergence of K and E at 550th iterations.

I have also done simulation with 1 million mesh and got the same result for K and E as K and E diverges at a particluar point in simulation and never converges.

Mohsin

 -mAx- July 29, 2010 03:04

This is not divergence.
Let iterate.

 Mohsin July 29, 2010 03:25

1 Attachment(s)
After almost 9500 iterations for 1 million mesh. I got the following residulas with under relaxation for Pressure=0.35, momentum=0.6 and K and E equal to 0.5 each. Its confusing. (why increasing the mesh size from 0.21 million to 1 million caused even the continuity and velocity residuals to diverge keeping all other factors same).

 Mohsin July 29, 2010 03:34

Quote:
 Originally Posted by -mAx- (Post 269285) This is not divergence. Let iterate.
Convergence Criteria
Contours
flux reports

In the previous case of 1200 iterations all were satisfied. Would you still recommend to iterate more? (if i iterate more the residuals for K and E will cross the convergence limit and never converge)

All times are GMT -4. The time now is 10:41.