[oozcan]

Hi all,

I am working on 3D heat exchanger flow and heat transfer.

First I have done first order schemes and got results in about 200 iterations.

But I have tried to continue in second order but still continuity residuals havent been enough down

How can I resolve it?

Mesh statictics and fluent residuals are attached.

Kind Regards,

[CeesH]

why do they need to go down more?

[oozcan]

Originally Posted by CeesH

why do they need to go down more?

Because that is not still converged.

[CeesH]

On what fact do you base that your simulation is not converged? Can you give me your criterion to judge convergence?

[oozcan]

Originally Posted by CeesH

On what fact do you base that your simulation is not converged? Can you give me your criterion to judge convergence?

as far as I know if each residuals go down about 10-2 Then for example iteration 101 is converged like that writing comes up in fluent box.

in first order schemes there is no problem I have run across because that was converged in about 200 iterations.

to get better results i have tried it in second order schemes,and you see what it like,

I have defined coupled and the other options are second order

The other way around I have activated k-epsilon ( realizable and standart pressure because y+ is too small value and activated energy equations to see heat transfer and flow )

and in materials gas is defined in polynomial function.

That is the final situation you have seen attached(photo) and still doesnt come up converged writing in fluent box.

Can you share me if you know something but I know a thing ?

Kind Regards,

[CeesH]

But the fact that the 'converged' writing comes in the FLUENT box doesn't really mean anything - it only means that the solver met the criteria that you said it should meet. If those criteria are too weak, it may say it converged while it did not. If the criteria are too stringent, your solution may have actually converged for all practical purposes, but the solver will not stop. So that's why I'm asking you on what basis you decide what 'converged' is. Only the residuals won't tell you - they give a trend in convergence, but do not tell you about the quality of your solution in the absolute sense.

[oozcan]

Originally Posted by CeesH

But the fact that the 'converged' writing comes in the FLUENT box doesn't really mean anything - it only means that the solver met the criteria that you said it should meet. If those criteria are too weak, it may say it converged while it did not. If the criteria are too stringent, your solution may have actually converged for all practical purposes, but the solver will not stop. So that's why I'm asking you on what basis you decide what 'converged' is. Only the residuals won't tell you - they give a trend in convergence, but do not tell you about the quality of your solution in the absolute sense.

you mean if all residuals are in a trend ,that is like something converged.Because all trends try to tell us something like way towards to going down or something.

The reason why I havent still seen converged writing is that criterias I have defined are stringent.

Accordingly, there is no problem in that solution and you say you keep it up and go see it in CFD-Post

is that right?

Kind Regards,

[CeesH]

What I mean is that your residuals indicate whether or not your solution is getting better or worse compared to your initialized flowfield, but they do not directly tell how much better or worse. It depends on the initial guess, on the parameter you check, on the geometry of the domain, and so on, how much your residuals will need to drop before you can say the solution is converged. So, based on the residuals alone, you can never say your simulation has converged. You will need to check something else.

You can plot for example the volume average velocity, temperature, the drag coefficient, the averaged wall nusselt number, depending on the parameters you are interested in. If these parameters reach a steady value (within a certain margin of error), you can conclude whether or not your simulation converged.

[oozcan]

Originally Posted by CeesH

What I mean is that your residuals indicate whether or not your solution is getting better or worse compared to your initialized flowfield, but they do not directly tell how much better or worse. It depends on the initial guess, on the parameter you check, on the geometry of the domain, and so on, how much your residuals will need to drop before you can say the solution is converged. So, based on the residuals alone, you can never say your simulation has converged. You will need to check something else.

You can plot for example the volume average velocity, temperature, the drag coefficient, the averaged wall nusselt number, depending on the parameters you are interested in. If these parameters reach a steady value (within a certain margin of error), you can conclude whether or not your simulation converged.

So, I have a just one question about URF. What does URF effect in congerved criteria.I have read some post in CFD-Online.and someone posted sum of pressure and momentum are equals 1 . Whereas momentum and pressure in URF 0.75, 0.75 respectively as default.After I read that post, I changed momentum 0.2 and pressure 0.8

Can you help me with that ? I have some confussed.

Kind Regards,

[CeesH]

There is no need to let those two equal to 1. URFs make the changes between your iterations smaller by blending part of the new solution with part of the previous, basically. The lower the URFs, the more stable the solution becomes, but the slower it convergence since the change per iteration is smaller. So if you can keep your URFs high and the residuals steadily go down/your solution parameters reach a steady value, keep them high. But if your residuals and simulation averages start oscillating and do not converge, you may wish to lower them.

[oozcan]

Originally Posted by CeesH

There is no need to let those two equal to 1. URFs make the changes between your iterations smaller by blending part of the new solution with part of the previous, basically. The lower the URFs, the more stable the solution becomes, but the slower it convergence since the change per iteration is smaller. So if you can keep your URFs high and the residuals steadily go down/your solution parameters reach a steady value, keep them high. But if your residuals and simulation averages start oscillating and do not converge, you may wish to lower them.

Grateful thank you,

and last one you mean lower the URFs the more stable the solution how much I decrease that values? for example 0.1 or 0.05 and what maxmimum value is needed? 1 or above 1 ? or 0.95

Kind Regards,

[CeesH]

Depends very much on the problem. If you have strongly recirculating flows, you may want to decrease the momentum URF to 0.2 or so due to strong non-linear effects. In a straight pipe flow, the default values should be sufficient. So it is a matter of experience; the higher you can keep them the better, but if you notice oscillation, gradually release them. I wouldn't go under 0.1 typically; if your results still oscillate then it is more likely your mesh quality of physics setup is problematic (and you do have some high skewness it seems - so that could play a role. Improving your mesh quality would not be bad).

[oozcan]

Originally Posted by CeesH

Depends very much on the problem. If you have strongly recirculating flows, you may want to decrease the momentum URF to 0.2 or so due to strong non-linear effects. In a straight pipe flow, the default values should be sufficient. So it is a matter of experience; the higher you can keep them the better, but if you notice oscillation, gradually release them. I wouldn't go under 0.1 typically; if your results still oscillate then it is more likely your mesh quality of physics setup is problematic (and you do have some high skewness it seems - so that could play a role. Improving your mesh quality would not be bad).

I am so grateful for your help,

I am studying master's degree and that is my dissertation.This project is consist of external flow around tubes and internal flow in tubes.you have just told default parameters are enough for pipe flow and that is more outstanding information for me.For a steady solution I have to try a bit small values ( 0.60 and 0.60) lower than default values ( 0.75 and 0.75) maybe um, iterations could be more much as a default parameters.But solution it will give me more stable,

Thank you for all

[CeesH]

Good luck! And don't forget to monitor the mean velocity and so, to see whether or not your solution reaches a steady state!

C

[oozcan]

Originally Posted by CeesH

Good luck! And don't forget to monitor the mean velocity and so, to see whether or not your solution reaches a steady state!

C

Hi again

Maybe um, you would help me as you can see the post.

the photos I have uploaded show that some recirculating, right?

That's why I need to change momentum in URFs about 0.2 as you told me as a recommendation.

This post is result of first order upwind schemes.I have activated standart pressure in k-epsilon turbulence model because y+=30 in internal flow and y+=1 in external flow.Standart pressure is defined in laminar fluid flow zone (1<y+<4 ).But I have two different y+ boundary conditions.I couldnt change both y+ values as two fluid flow zones has different velocity and diameter/hydrolic diamater.

Kind Regards,

[CeesH]

So did you check how your monitors (av. velocity vs. iterations or so) behaved? Did you reach a steady state? If so, then we can look at how good the results are. If they were still oscillating then we have to consider why that happens first.

[oozcan]

Originally Posted by CeesH

So did you check how your monitors (av. velocity vs. iterations or so) behaved? Did you reach a steady state? If so, then we can look at how good the results are. If they were still oscillating then we have to consider why that happens first.

I have just checked velocity magnitude and that is not completely realistic( I have changed momentum 0.2 not to see recirculating flow).Actually I havent seen where mean velocity were.Anyway velocity magnitude should need to be about 6 m/s as I have calculationed all projected manually it

As for reaching steady-state , I think all residuals compared to initiatiated boundary conditions has gone down similarly regimes.But I dont think that is reaching steady-state as velocity magnitudes is not even close

Last one is Vortex emerged more than the former one after I changed momentum in URFs as 0.2

Kind Regards,

[CeesH]

Ok, but can you go to monitors > volume monitors and set a monitor for volume averaged velocity? Tick the 'plot' option. Then it will be plotted similar to the residuals, and you can see whether it becomes stable or not.

We are not talking about realistic values now - the question is whether or not your solution converged. If you do not know if your solution converged, you cannot comment on how realistic the values are.

[oozcan]

Originally Posted by CeesH

Ok, but can you go to monitors > volume monitors and set a monitor for volume averaged velocity? Tick the 'plot' option. Then it will be plotted similar to the residuals, and you can see whether it becomes stable or not.

We are not talking about realistic values now - the question is whether or not your solution converged. If you do not know if your solution converged, you cannot comment on how realistic the values are.

Thank you

I got what congerved means,

I have done averaged volume velocity in volume monitors but I can't see save output parameter (https://www.sharcnet.ca/Software/Ans...r_volumes.html)

Then, I have to look at results > reports> volume integrals then I have saved output parameter on my desktop then I have entered XY plot and loaded that file to select all surfaces in XY plot dial box and now it is writing. is it all right?

On the other hand I try to make mesh in multizone

But in the volume integers, defined averaged volume velocities are about 10% more than manual calculations

you can see attached photo

Thank you

[CeesH]

but what you show now are instantaneous values, you cannot draw any conclusions based on those; you need to know if they are stable over a number of iterations, to see whether or not your solution converges.

Consider this image for the drag coefficient for example (from LionTech Rockets Laboratories); you can see the drag coefficient reaches a steady value after about 300 iterations. So, after 300 iterations the simulation converged (depending on your specific demands of course, and you will need to monitor a bit longer to see whether or not it stays stable)

So did you make a similar plot for your setup, with velocity, or temperature, or whatever parameter - as long as it is of interest for you. If not, do so. It is under monitors > volume average, tick plot and set the window where you want to plot. You can write to file and load it in excel or matlab too, but just plotting and watching is easier.