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

What do you mean by this? You can't really tell if a solution is converged just by looking at the residuals.

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.

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.

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
*is your set up in agreement with physics of your model? (laminar instead of tubulent, unsteady instead of steady, compressible instead of uncompressible, etc...etc...etc...)

Thank you for your answers/suggestions.

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.

Please help me in this. I wil be grateful.

Mohsin
South korea.

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.

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

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

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.

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

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?.....

*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

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.

Awaiting your valued comments.
Mohsin

This is not divergence.
Let iterate.

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).

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)

Ok here it diverges :D
Well without the model I can't do more (and I don't have Fluent)
:rolleyes:
Try to switch with unsteady solver

Brrrrrrrrr

Well. I think i have to invite you here to South Korea to solve this one:)

Lets nap first and then think about some solution:)Thanks anyway....
Mohsin

hi mohsin,
it has been a year since your message. but i have a similar problem amd i would be glad if you could tell me how did you manage to solve this problem?

Please explain your problem....
Are u seeing residual rise in your solution?

yes. residuals decrease until 0.1 or 0.01 for 500~ iterations and then continuity strarts increasing and it diverges (e20 or so) at 1500~ iterations.
now i decreased URFs a lot and got a converged solution. i will try increasing URFs step by step.
so you have any other suggestions?
i am only solving turbulent flow and using k-epsilon model (realizable).
thanks already

Hello Riccia

Suggestions for you:

1. If the residuals rise (for example, first converge and then start to diverge) then wait for some iterations to see whether they converge again or not. If the resiudals don't converge and keep on diverging then there is a problem. The problem (MOSTLY) comes from poor mesh quality. Go back and try to improve your mesh quality. Use hexahedral meshes and avoid tetrahedral meshing scheme unless u have a very complex geometry. Mesh quality should be as follows for 3D.

a. Skewness for Hexahdral mesh elements should not exceed 0.8.
b. Skewness for tetrahderal elements should not exceed 0.85.

2. if the residuals keep on diverging, You SHOULD NOT change the URF to a very low value. If you change it to a very low value then apparently the solution would converge but it wont be accurate. For example you may not reduce the URF for momentum to 0.1 0r 0.01. If you use this value for momentum then the solution will drastically jump to convergence criteria specified by u. However, the solution would be wrong and inaccurate. So, at first, try to use the same URFs as provided by FLUENT (Default). If you get fluctuations then it means you have to change some urf to get steady lines. The following URF values mostly work for me.

a. Presure: 0.4
b. Momenutm: 0.6
c. Turbulent kinetic energy=0.6
d. Turbluent dissipation=0.6
e. Rest=Default

3. Discretization scheme: Use of discretization scheme may also affect. Choose the best discritization scheme for ur problem which do not give you divergence. for example: If swirl is there in ur flow then i would recommend PRESTO scheme.

4. Turbulence scheme: You may also try to find appropriate scheme for turbulence in order to get steady converged solution.

5. last but not least, Residulas are not the only convergence criteria. For instance, if your residulas are not going below 10-3 then let it be there and check the mass flux (in and out) if the valuesof total mass flux in and out are (for example) lesser than 10-4 then your solution might be converged.You can also monitor the surface intgrals on some point of importance in ur domain and call ur solution converged when the value is not changing.

Keeping in view the aforementioned points, try to solve your problem. I hope you will get a solution.

Good luck

I have the same problem, somehow. The residuals are decreasing for the first 700 iterations to about 1e-4 but then suddenly it increases to about 1e+2. After following your problem here, I have ended up with your last post which is still a problem without any solution.

I am wondering whether you have solved the problem?? if yes, could you kindly post here what steps you took??

Or, is there anyone here who can help??

Thank you in advance

Sorry for the previous message, in fact I got access to the rest of the conversation (on the other page) right after posting the message.

Anyway, I got your suggestions. I have implemented most of them but did not lead me to a converge solution yet. Now, I will try to refine the mesh size even though the mesh quality for the current case is relatively good. Hopefully I will manage to get a good converged solution if not then I would most probably need your help!

Hi.
I am modeling a open channel flow.
What the problem of this residuals?
Can you tell this is going to diverge or not?
please see image
thanks

hi Mohsin
I'm master student and work on swirl flow . i have problem like your's would you pleas help me if you solve your problem.
thank you

Many have already answered to this question.
You should monitor the interested quantities to understand if the solution converged or didn't.
Anyway having continuity residual of 10e-2 order is too high from my experience.
In this cases check the BC, it can be generated by recirculations on outlet.