Hi,

I get a steady state solution for a diffusing bend when the mesh is coarse. However, I start getting some unsteady solution when I refine the near wall mesh (O grid type is used). The pressures & velocities that I monitor at some locations inside the domain show small fluctuations along the mean values (say +/-0.2Pa at mean value of 125Pa)and the max momentum residuals stay at the order of 10^-2 (around the same magnitude for both 3) P-max residual stays at the order of 10^-4. RSM, SST, kw, SSG, RNG ke models all show similar phenomenon (except for standard ke).

What should I do about this situation? Should I stick with coarse mesh solution? Can I use this unconverged solution? I will need the steady state solution to run the transient simulation later.

Thanks for any help here.

i do not have cfx but in fluent i usually export the results from the coarse mesh and then import these results in finer mesh as initial guess, results do converge very quickly.

sometimes fine mesh could slow down convergence, but cfx i think this should not create much problem. the other cfx users might tell you how to export the initial guess from coarse to fine if possible.

Hi,

Thank you for your comments. I've already extrapolated the coarse mesh solution onto the fine mesh definition file before I start the solver. The max residual will drop rapidly in the first 100 iterations but stay at about same level (with small oscilation, sort of like a noise) thereafter (I run totally 3000 iterations and there's no sign of convergence and residuals just stay almost the same).

This situation just happen when I start refining the mesh close to the wall (O mesh is used). I found out that I can only reduce the first node distance to a certain value. If I define a smaller value than this, I will get the convergence problem as stated in the first post regardless of whether I'm using omega- or epsilon-based model. Surprisingly, standard ke model doesn't seem to have problems reaching the target max residual (5e-6).

I believe this is not a new problem for simulation. Please kindly give me some more feedback if possible.

Do you think increasing turbulent dissipation artificially will help the convergence here? If so, what method will you use to do this?

1) Monitor ur maximum residual locations..2) when u refine u may find it capture more physics, it could be unsteady state by nature !!

HK

Hello,

I experience similar behaviour in my calculations. You could output the residuals to the .res- file and have a look where the large values are located in your domain. If they are located in small areas only, the results may be meaningful in spite of the high residuals. Also try to monitor a quantitiy being characteristic for your problem and look whether or not it changes while iterating.

Generally, it seems that with refined mesh, reaching convergence gets harder. This may be due to the fact that transient effects come into play which cannot be captured using coarse meshes. I don`t think that increasing turblent dissipation would be a good way to resolve the problem because it would to a certain extend corrupt the advantages from refining the mesh. If transient effects are important, then the only solution is to do a transient calculation.

HTH,

Thomas

Try reducing your timestep (so that the courant number is obeyed)

Hi Thomas,

Thanks for your help. Yes. I've already plotted out the isovolume of the residuals in post. Some of the worst residuals are located inside my domain of interest and they are quite close to the wall (not in the middle, just around the centre if you get what I mean). As I'm going to study the transient losses inside the diffusing bend later, it may be a problem if the residuals are large near the wall (Not sure at this stage though, anyone has the similar experience please kindly give some advices...may have to carry out some more experiments to check this out)

As I mention before, I've put a few monitoring pts to check the velocities and static pressures at the centre of several cross sections inside the domain. They're not converging nicely to a single value like the coarse mesh solution. The pressure values are not changing much but fluctuate about the mean value (e.g +/- 0.2Pa about 125Pa). This phenomenon stays for more than 1000 iterations and so I don't think it will finally converge even if I specify more iteration steps. Not sure what the solver is trying to hunt for. I do the same observation in the coarse mesh solution. There's no pressure fluctuations and the pressures/velocities are converged to a single value.

For the physics, I expect some flow separation to occur at the upper surface. It's a diffusing bend and secondary flow may develop in the domain.

If transient simulation may solve the problem, then what initial file should I use? The well converged coarse mesh solution or the unconverged fine mesh solution? The transient simulation always need a good steady state solution to start with. Isn't that right?

Thanks for help. I remember that I've run a transient simulation with constant BC before but the solution isn't converged well. I only use the SSG model for the trasient simulation so far. The boundary condition is quite simple. Constant total pressure at inlet,smooth wall and constant static pressure at outlet. 5% TI. I believe there must be a trick to overcome this but I just don't know it right now. Any suggestions will be most welcomed.

You mean the timescale control? I always use the automatic timescale. Try reducing it manually before but doesn't have much effects on the convergence. Thanks anyway.

i can't really comment much on this , but the convergence is one this i must point out that convergence doesn't really mean that if your residuals are around say 10^-6 you got the convergence if the solution is changing, in other words since residual is global sum, the individual values may be changing. so if we decide that convergence is when the individual values top changing, we say that convergence is reached (to the extent possible in present situations), the global residual may be high as 10^-2.

what i want to say is after a limit the values shal become constant and thus the global residual also stays at that value. for this reason lot of people monitor the values at some particular point, to see if the values are changing there or have become stable and use this as cretiria.

Thanks again. I see your point. That's exactly what I'm talking about here. The max residuals drop to a certain level and will not drop further even though thousands of iterations are assigned (ideally the residuals should converged to machine round-off error)

When the residuals aren't converged, I double check it with the pressures/velocities values at some monitoring pts and found that the values are changing up and down (magnitude of fluctuation is small) till end of the max iterations assigned (sort of like small sinunsoidal oscillations about a mean velocity/ pressure value). Is that the transient effect that you guys are talking about here? Is there a trick to overcome this?

i am not sure what timesclaes they are talking about, but what i want to say will be more clear by reading this. This is what Fluent manual says:

[[[[[ From manual:

Implicit solution of the linearized equations on unstructured meshes is complicated by the fact that there is no equivalent of the line-iterative methods that are commonly used on structured grids. Since direct matrix inversion is out of the question for realistic problems and "whole-field'' solvers that rely on conjugate-gradient (CG) methods have robustness problems associated with them, the methods of choice are point implicit solvers like Gauss-Seidel . Although the Gauss-Seidel scheme rapidly removes local (high-frequency) errors in the solution, global (low-frequency) errors are reduced at a rate inversely related to the grid size. Thus, for a large number of nodes, the solver "stalls'' and the residual reduction rate becomes prohibitively low.

The multi-stage scheme used in the coupled explicit solver can efficiently remove local (high-frequency) errors as well. That is, the effect of the solution in one cell is communicated to adjacent cells relatively quickly. However, the scheme is less effective at reducing global (low-frequency) errors--errors which exist over a large number of control volumes. Thus, global corrections to the solution across a large number of control volumes occur slowly, over many iterations. This implies that performance of the multi-stage scheme will deteriorate as the number of control volumes increases.

]]]]

what you are talkig about this the effect where we call the solver "stalls", that is it stops to remove the erros from the solution, and manual also mentions how coupled solvers stall for low frequency erros (exist on global level). so to over come this problem, we need multigrids. Now, i assume that the solver you are using is coupled multigrid solver, in this case, if you are facing the problem they have mentioned, you can try these things:

1. increase the number of multigrid levels

2. try to increase the number of iterations it perfoms at each level.

Hi,

You're right. CFX employs multigrid coupled solver to accelerate the convergence. I never increase the number of multigrid levels before and have assumed the default settings will always work fine. Have to check if there is any such option in CFX. Unfortunately, CFX doesn't use the segregated method and so I can't test it out here. Thanks again for digging out the literature from Fluent user manual.

well i din't dig the manuals, its just that i remember what they have written so just pasted it here, further about segregated approach, in a k-omega model with mesh size around 4.5 million cells i do get convergence of order 10^-6 for continuity. i only use coupled solvers with coarse meshes to generate initial guess for such large size cases since other wise k-omega model usually do not converge at all, they are pretty stiff set of equations.

and one more thing, the original k-omodels by wilcox is sensetive to boundary conditions, so the k-omega model in fluent is a little bit different from k-omega model of wilcox , so you may want to look into the k-omega model used by cfx, how they employ it.

Thanks for the info. Your test case is very useful for my problem. I'm strive to get some experimental profile for this problem as well. The inlet is open to atm and so the constant total pressure shouldn't work too bad in this case. I use the outlet wall static pressure measured at several outlet locations as the BC. Hence, I don't think I'm too far away from the real physics anyway. Both Inlet & Outlet locations have been extended some distance away.

Just to summarise some approaches that I've tried so far for the SSG model (I did use other models on the same mesh setup and show similar convergence problem on fine mesh, except standard KE model. However, KE model doesn't show satisfactory result for diffusing bend). Note that I didn't change any constant for the models. Just use the default one.

For case 1 & 2, solution converge to target residual (5e-6) without problems (for all turbulence models tried in CFX). All pressures & velocities at monitoring points are converging to a single value smoothly.

For case 3, I just add ONE MORE nodes in the direction normal to the wall (O grid) and residuals start to show problem going down. Instead they stay at the same level for more than 1000 iterations. Pressures & velocities at some monitoring pts show small oscillation and just don't want to settle down. I look at the Y+ value, it's still very well above the sublayer zone for majority of the region. Same thing happen for w-based model. I don't see why this approach has such impact on the convergence anyway.

Case 4 is the fine mesh where I increase the nodes on all the edges. Needless to say, it didn't converge.

Case 1- Original Coarse Mesh Average Y+=146.091, Max Y+~253

Case 2- Refine the mesh in the middle region, near wall mesh remain the same: Average Y+=148.594, Max Y+~258

Case 3- Refine only need wall mesh: Average Y+=125.046, Max Y+~224

Case 4- Refine the mesh in all directions: Average Y+=96.1279, Max Y+~177

For the mesh, ICEM show a min quality of 0.64 & only less than 50 elements has quality less than 0.7. Min angle ~40. I consider this as sufficient for most solvers.

Hello TB,

I wasn't exact enough when I mentioned monitoring of variables. From your posts I learn that you are interested in the losses ocuring, so probably try to monitor this quantity (this was meant by saying "monitor a quantitiy being characteristic for your problem"; normally, one is not interested in the value of a flow variable at one single point of the domain but rather in integral values) and look at its behaviour. Anyway, I would not worry too much about such a small change in the pressure at a single point in the domain.

I have done a flow calculation of a fan with a diffusor attached and also had problems with high residuals. Doing a transient calculation using the steady state solution as starting point solved the problem for me. The residuals reached at each time step were about 3 orders of magnitude lower than at steady state. However, the simulation had to run for some time because the starting values obviously were not very good so that I had to do a lot of timesteps.

Hth

Thomas

Hi Thomas,

I run the transient simulation with w-RSM model this week. This method looks promising as what you said even though more than 60 iterations may require for each timestep. However, it doesn't apply to SSG model. I suspect this has sth to do with the wall function.

Anyway, thanks for sharing your idea with me.

[hello-fluenttt]

Hello friends
I have been doing the shock tube problem. when i had a coarse mesh, everything was fine, however now i want my mesh to be too fine so as capture exact shock wave as thin line( order of 10^-8m cell size) and also very small time steps, but the solution is too far from converging,. its 2d inviscid flow

any help would be apreciated
thanks

[hello-fluenttt]

Hello friends
I have been doing the shock tube problem. when i had a coarse mesh, everything was fine, however now i want my mesh to be too fine so as capture exact shock wave as thin line( order of 10^-8m cell size) and also very small time steps, but the solution is too far from converging,. its 2d inviscid flow
what should i do ????

any help would be apreciated
thanks

[Sasquatch]

What you are observing is correct. Densifying the mesh results in more unsteady convergence because you resolve also smaller terms in your domain.

I am not an expert but this trickles down to the statement that often densier mesh does not necessarily mean a better solution - a proper mesh independence study needs to be done to find an optimum.

In case you need it as an initial guess, a bad result is still a result, however, keep in mind that transient simulations are costly and in case of a bad initial guess, the solution will stabilize much later.

I hope I helped.