Hi all,

I am getting the error message "Turbulent viscosity limited to viscosity ratio of ... in ... cells"

What is the reason for that?

What is more important is, how to get a list of Fluent Error Messages and their descriptions, so that we will not have the same torture again and again each time facing the error messages??

Hi gun,

I have had that same problem. Most of the time it dissapears after a few iterations, about 100 or so, but sometimes I have to change the grid. If you are using wall functions check your Y+ values and make sure they are between 30 and 60.

Hopefully that will help.

Eric

Try to adapt the grid on isovalue, e.g adapt all cells where turbulent viscosity is greater than a specific value. Then run the case again.

When you see the message appear, stop the iteration and check the velocity field. I will bet that there are some cells with very high (unrealistic)velocities. Under relax things a bit, and keep iterating, the message should dissappear once the solution is more converged.

Alternatively...

go to

Solve>Control>Limits

and set the limit for turbulent viscosity to 1e20.

Then carry on iterating.

If turbulent viscosity is limited to 1e20, there is something wrong!

DAE

Alternatively...

go to ... Solve>Control>Limits

and set the limit for turbulent viscosity to 1e20.

Then carry on iterating.

If turbulent viscosity is limited to 1e20, there is something wrong!

DAE

i tried your suggestion in my case, it didn't work, what's wrong?

don't know... what are you modelling, what viscous model are you using, what is your grid size, boundary conditions etc etc.

I am simulating a tunnel with water flowing freely through it.the water is not full of the tunnel's section, and there is air upon the flow. there is a sudden fall in the middle of the tunnel so the water flowing along the floor becomes a jet flow, and then again falls on the floor and flows out of the exit. there are both free surface upon and under the water of the jet part and a large volume of air bubbles mixture into the water body.so I use mixture model to catch the concentration of air bubbles in the water and the location of free surface.(is that model suitable for this simulation? and other suggestions?)the domain I simulate is the whole tunnel and I divide the inlet into two: the upper one for air with pressure inlet boundary condition and the lower for water with velocity inlet. the outlet is defined as pressure outlet. Downstrean the fall, there are two side tunnels going straight up and connecting with atmosphere, so the entrances of the side tunnels are also defined as pressure inlet.I initialize the domain from the velocity inlet.At the beginning, I use lam and vof to get a easy-solve field, and then change to rke and mixture. Air and water are both treated as incompressible and the residuals are all set to 0.001.URF are all set to 0.1, discretization of pressure is body force weighted and p-v coupling is Piso, all others are first order upwind. the turbuluence viscosity ratio is limited to 10^5, and the absolute pressure is limited not less than 0. But not long after the computation, both the ratio and pressure exceed the ratio.so I raise the limit of ratio to 10^10, but after some iterations there still some cells exceed. and then there occur regions with weird high velocity and pressure. about the grid size, the velocity of water is about 40m/s and to match the condition of using wall function, I use boundary layer to make y+ between 30 and 300, namely Ypis about 0.00015m. then the thickness of the grids raises 5 times of the adjacent ones near the wall.and the size of the central grids is about 1m*1m,the difference is huge.I think maybe the skewness of the grid is one reason to cause the problem. BTW: body force is included in my case.

Initial comments... for the inlet, make it a velocity inlet, and specify the fraction of phases at the inlet. If you have gravity on obviously they will seperate.

Change the turbulent viscosity limit to 1e20 before attempting any iterations.

Make sure that the maximum cell skewness is less than 0.85.

Try modelling just the water and air, and avoid trying to capture the bubbles until you have got the other to work.

I don't think the values of y+ or y* will effect whether you get convergence or not, but I could be wrong. If you have bad cells as a consequence of trying to get y* or y+ down, then forget about this for the time being. You can always adapt the mesh in fluent.

Does this help?

i agree with most of what you said, especially about the y* and y+.But from my experience, loosing turbulence viscosity ratio only make the convergence become easy, but the weird high velocity and pressure do not disappear. and another difficulty is that velocity inlet can't be used here, only pressure inlet left to be used.I am not sure how to set pressure inlet, especially when I initialize the field with water full of the whole tunnel.The altitude difference between the inlet and the outlet is about 84m, means there are 8 atms between them.Under such condition, I set the gauge pressure of outlet as 0, and the gauge total pressure of inlet as 0 too. and as i mentioned before, there are two windlet defined as pressure inlet, and they are lower than the air inlet and are different in height.I still set their gauge total pressures as 0. Is that right? In my opinion, both of the pressure inlets and outlet are connected with atmosphere, and their gauge pressure should be 0(the operating pressure is 1 atm).But there is 8 atms difference between the inlet and outlet at initial time,how could I explain and deal with this? And now I am wondering if it is this make convergence so difficult to reach and there occur so weird high pressure and velocity in the domain.Please give me some suggestions.Thanks in advance!

Why can't you use velocity inlet as the inlet condition?

Do you know the mass flowrate of water through the system?

Thanks

DAE

Yes, I know the flow rate of water, but I don't know the flow rate of air, nor the volume fraction of it.So the inlet of air should be defined as pressure inlet.

If you are not going to be looking at the capture of air bubbles for the time being, I think you should be using the VOF model, and i think for your case, geo-reconstruct.

DAE

I tried VOF, and the weird high pressure and velocity still occur, just like Mixture. Now I am thinking about that if it is the setting of pressure that makes this unpopular and unphysical phenomenon exist.Can you give some suggestions of pressure setting?When both pressure inlet and outlet are used, their locations different in height to 80m,and I use 0 gauge pressure on the pressure outlet and 0 gauge total pressure on the pressure inlet, is that right?

I think it is probably the pressure too, which was why i said use a velocity inlet for both the air and water and I think you should still try this.

To be honest, although you have taken some effort to explain, I don't realy understand what it is you are modelling, but is the air likely to have a velocity? If not, you could use a UDF to specify the velocity of the air and water seperately.

DAE

yes, I will try. In my last case, I used velocity inlet for air and didn't meet such trouble.So I think it maybe caused by pressure setting.Anyway, it is an interesting question to think about.If you have interest in it, I will email my case to you.Thanks a lot, you are a real friend.

could you e-mail your case to me? If you could zip it first, and as long as it isn't too big?

Thanks

DAE