CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLUENT

ERROR-Turbulent Viscosity Limited to ...

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   November 28, 2003, 05:58
Default ERROR-Turbulent Viscosity Limited to ...
  #1
gun
Guest
 
Posts: n/a
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??
  Reply With Quote

Old   November 28, 2003, 06:16
Default Re: ERROR-Turbulent Viscosity Limited to ...
  #2
eric
Guest
 
Posts: n/a
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
  Reply With Quote

Old   November 28, 2003, 07:40
Default Re: ERROR-Turbulent Viscosity Limited to ...
  #3
-
Guest
 
Posts: n/a
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.
  Reply With Quote

Old   November 30, 2003, 18:52
Default Re: ERROR-Turbulent Viscosity Limited to ...
  #4
Anton
Guest
 
Posts: n/a
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.
  Reply With Quote

Old   December 4, 2003, 12:32
Default Re: ERROR-Turbulent Viscosity Limited to ...
  #5
DAE
Guest
 
Posts: n/a
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
  Reply With Quote

Old   December 4, 2003, 12:32
Default Re: ERROR-Turbulent Viscosity Limited to ...
  #6
DAE
Guest
 
Posts: n/a
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
  Reply With Quote

Old   December 11, 2003, 12:45
Default to dae
  #7
richard
Guest
 
Posts: n/a
i tried your suggestion in my case, it didn't work, what's wrong?
  Reply With Quote

Old   December 12, 2003, 05:53
Default Re: to dae
  #8
DAE
Guest
 
Posts: n/a
don't know... what are you modelling, what viscous model are you using, what is your grid size, boundary conditions etc etc.
  Reply With Quote

Old   December 16, 2003, 01:45
Default Re: to dae
  #9
richard
Guest
 
Posts: n/a
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.
  Reply With Quote

Old   December 16, 2003, 06:18
Default Re: to dae
  #10
DAE
Guest
 
Posts: n/a
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?
  Reply With Quote

Old   December 16, 2003, 10:51
Default Re: to dae
  #11
richard
Guest
 
Posts: n/a
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!
  Reply With Quote

Old   December 16, 2003, 13:51
Default Re: to dae
  #12
DAE
Guest
 
Posts: n/a
Why can't you use velocity inlet as the inlet condition?

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

Thanks

DAE
  Reply With Quote

Old   December 16, 2003, 22:28
Default Re: to dae
  #13
richard
Guest
 
Posts: n/a
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.
  Reply With Quote

Old   December 17, 2003, 10:22
Default Re: to dae
  #14
DAE
Guest
 
Posts: n/a
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
  Reply With Quote

Old   December 18, 2003, 05:01
Default Re: to dae
  #15
richard
Guest
 
Posts: n/a
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?
  Reply With Quote

Old   December 18, 2003, 09:37
Default Re: to dae
  #16
DAE
Guest
 
Posts: n/a
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
  Reply With Quote

Old   December 18, 2003, 10:14
Default Re: to dae
  #17
richard
Guest
 
Posts: n/a
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.
  Reply With Quote

Old   December 19, 2003, 07:12
Default Re: to dae
  #18
DAE
Guest
 
Posts: n/a
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
  Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
reversed flow at pressure inlet and turbulent viscosity is limited.... cfdiscool FLUENT 10 June 10, 2015 06:15
Turbulent viscosity limited to viscosity... Cyril FLUENT 16 October 4, 2007 06:12
Turbulence viscosity limited Madhukar Rapaka FLUENT 0 June 26, 2006 03:17
Turbulent viscosity limited to viscosity ratio... Cyril FLUENT 8 February 7, 2006 21:34
Problem of Turbulent Viscosity Ratio Limited David Yang FLUENT 3 June 3, 2002 06:13


All times are GMT -4. The time now is 05:36.