[the_sixth_hokage]

Hi..

I'm modelling a species transport of LOX methane under 5.6MPa (transcritical conditions)..I'm using Eddy dissaption concept..

I have cold run the initial for and after reaching a good starting point I switched on the combustion.

The residuals seems to go down and no turbulence warnings appear for some iterations (about 100 itrns)..

All of a sudden the turb viscosity warnings appear and increase in a significant amount of cells and residuals starts increasing...and finally gets diverged.....

I am using a coupled solver ( with first order for initial solution). My urfs are very low..(turb viscosity - 0.2)

Please help

[vinerm]

Which turbulence model are you using? k- is known to overpredict k under certain circumstances leading to very high eddy viscosity. You may also enable production limiter to limit the production of k. This may help to an extent. Do not use such small URF for eddy viscosity. You have to monitor if the number of cells with high turbulent viscosity are increasing or decreasing. They would, of course, increase in the beginning but will reach a dwell point and then start reducing. If that is the scenario, then you don't have to worry about. If that is not the case, then you have to check your turbulence model, and mesh size and quality.

[the_sixth_hokage]

Originally Posted by vinerm

Which turbulence model are you using? k- is known to overpredict k under certain circumstances leading to very high eddy viscosity. You may also enable production limiter to limit the production of k. This may help to an extent. Do not use such small URF for eddy viscosity. You have to monitor if the number of cells with high turbulent viscosity are increasing or decreasing. They would, of course, increase in the beginning but will reach a dwell point and then start reducing. If that is the scenario, then you don't have to worry about. If that is not the case, then you have to check your turbulence model, and mesh size and quality.

hi I'm using k epsilon model...I will try production limiter..

I initially do a cold run (by switching off volumetric reactions) and run till a good residuals ( even tried a converged) are obtained..the no of cells in which turb viscosity are below 4000...

When I switch on volumetric and patch a high temperature to start combustion the turbulence viscosity warnings go down and disappears completely and I get some good residuals...

After next 200 iterations or so the turbulence starts showing and increase rapidly and the residuals also starts going upto e+08 ,e+12 etc.. and finally diverges..


As for my mesh...I have a relatively simple 2D geometry...they geometry is rectangular cross section of a combustion chamber with rectangular block like inlets...

My mesh is well refined near my area of interest and has no skewness..

[vinerm]

Production limiter might help but does not always. As far as mesh is concerned, quality is one thing. But a mesh more refined than required tries to predict turbulent scales that a RANS model may not be able to handle. Therefore, ensure that the mesh is not very fine. This increases the source values in cells, because cells are very small, and the resulting matrix is no longer diagonal dominant, leading to divergence.

[the_sixth_hokage]

Originally Posted by vinerm

Production limiter might help but does not always. As far as mesh is concerned, quality is one thing. But a mesh more refined than required tries to predict turbulent scales that a RANS model may not be able to handle. Therefore, ensure that the mesh is not very fine. This increases the source values in cells, because cells are very small, and the resulting matrix is no longer diagonal dominant, leading to divergence.

So should I use LES models...is it possible to do LES models in combustion at transcritical conditions...I'm no expert on how to do a LES model!!

[vinerm]

I don't recall any compatibility issues between LES and EDC or Real Gas. However, LES may not be required for the case. You can continue to work with RNG or Realizable k-.

[the_sixth_hokage]

Originally Posted by vinerm

I don't recall any compatibility issues between LES and EDC or Real Gas. However, LES may not be required for the case. You can continue to work with RNG or Realizable k-.

Hey I tried the production limiter and it helped in reducing the no of cells to a significant amount..thanks..

But even when the no of cells are low I am facing divergence..

I made my mesh size larger and used all k-epsilon models( standard, rng and realizable)..

I use 1 chemistry iterations per 10 iterations..



The problem is...for a few iterations everything seems fine (for 90 iterations)..when the next chemistry integration kicks in I see a huge increase in energy, velocity, k, epslion and momentum residuals..

The energy residuals spikes and reach 10e+30 and higher and so does others too... finally gets diverged...

Since I'm using a custom Chemkin file, I switched to Fluent library methane-oxygen two step...still this problem occurs...

[vinerm]

This is happening due to very high energy source. Check the reactions, enthalpy of formation, and specific heats. If those are not appropriate, energy generated due to reaction would be extremely high and lead to divergence.

[the_sixth_hokage]

Originally Posted by vinerm

This is happening due to very high energy source. Check the reactions, enthalpy of formation, and specific heats. If those are not appropriate, energy generated due to reaction would be extremely high and lead to divergence.

Hi I checked the enthalpy , reactions and other factors...the units are correct and the chemkin files are imported correctly..my materials are good...

But I still get a huge peak in energy within 100 iterations...I tried different turbulence models...and different mesh sizes...

Everytime the reactions go fine until the 89th iteration the energy and continuity residuals explode ( in the range of e+30 )..the finally diverge..

I even tried with the default materials provided in the Fluent library...it also explodes near this region..


I am modelling a combustion of liquid oxygen(85 K) and methane(288 K) at transcritical conditions..

[vinerm]

Are you using a real gas model for this work? If yes, then you may have to provide a really good initial guess, most likely on the basis of ideal gas solution. So, you have to run an ideal gas solution first and then switch to real-gas.

[the_sixth_hokage]

Originally Posted by vinerm

Are you using a real gas model for this work? If yes, then you may have to provide a really good initial guess, most likely on the basis of ideal gas solution. So, you have to run an ideal gas solution first and then switch to real-gas.

Yeah I'm using SRK real gas equation..I'm setting the thermal conductivity and viscosity of the mixture to mass average mixing..and using the rest as default values.. I am also using the default fluid values too...

[vinerm]

Real gas models are difficult to converge. If you start the simulation directly with real gas model, it will not work. You have to use ideal gas, run the simulation until it reaches a stable state and then switch to real gas. You also need to ensure that the density of ideal gas is closer to the real gas you would be using.

[the_sixth_hokage]

Originally Posted by vinerm

Real gas models are difficult to converge. If you start the simulation directly with real gas model, it will not work. You have to use ideal gas, run the simulation until it reaches a stable state and then switch to real gas. You also need to ensure that the density of ideal gas is closer to the real gas you would be using.

Hi I ran an ideal gas model and got converged..then I switched to SRK model...but it diverged within 10 iterations..

I am not sure what you meant by density of ideal gas being close to my real gas model...how can I change the density... My test case has provided me with density of methane and oxygen at 5.6MPa..should I use this values and how??!

[vinerm]

The solution to be run with ideal-gas is only meant to provide a good initial guess for real-gas. However, if the density of ideal gas is very different from the real gas, the the solution from ideal gas won't be very helpful. If you already know the density range for the real gas, you should modify molecular weight for the ideal gas to match the density. Then the ideal gas solution would be helpful.

[the_sixth_hokage]

Originally Posted by vinerm

The solution to be run with ideal-gas is only meant to provide a good initial guess for real-gas. However, if the density of ideal gas is very different from the real gas, the the solution from ideal gas won't be very helpful. If you already know the density range for the real gas, you should modify molecular weight for the ideal gas to match the density. Then the ideal gas solution would be helpful.

Hi I did an initial solution with changed molecular weight...but when I switch back to SRK model I get mass imbalance errors...I even changed the values to default molecular weights...

Even when I ignore and run iteration, I get Analytical Jacobian not available for selected density...

[the_sixth_hokage]

Originally Posted by vinerm

Are you using a real gas model for this work? If yes, then you may have to provide a really good initial guess, most likely on the basis of ideal gas solution. So, you have to run an ideal gas solution first and then switch to real-gas.

Hi I managed to switch to SRK (ignoring the mass imbalance, but my reaction and stochimetric coefficients are good ) the energy and continuity residuals still gets spiked to 1e+7 and increasing...

[vinerm]

Fluent calculates analytical Jacobian for volumetric reactions but usually these are not required if there are no wall/surface reactions or until volumetric reactions are applied at a boundary.

If the case works fine with ideal gas and is giving trouble with real gas, then most likely everything is set up appropriately. The only thing that can help now is numerics. So, you may have to play with schemes and URFs.