CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   FLUENT (https://www.cfd-online.com/Forums/fluent/)
-   -   turbulent viscosity limited to viscosity ratio (https://www.cfd-online.com/Forums/fluent/106843-turbulent-viscosity-limited-viscosity-ratio.html)

 Alex_B September 10, 2012 15:11

turbulent viscosity limited to viscosity ratio

1 Attachment(s)
Hello, dear all!
May be you can help me!

-2D case, Mixture model, k-e standart viscosity
-cilinder with little adding inside (see picture Снимок.jpg)
-there is mixture inside cilinder (air volume fraction 0.95 + water 0.05) (like spray)
-velocity inlet 5m\s and Initial gauge pressure is 10000000 Pa (turbulence: intensity and visc.ratio 5 and 5)
-pressure outlet 9992500 Pa (turbulence: intensity and visc.ratio 5 and 5)

And again and again I have messages like:
reversed flow in 255 faces on pressure-outlet 11.

turbulent viscosity limited to viscosity ratio of 1.000000e+08 in 43005 cells

and after this

Error: Divergence detected in AMG solver
Error Object: #f

I try to implement all advices from this forum, but I have this bad massages.
So I suggest, that my problem in aerosol model. May be I implement wrong viscosity model or something like this.

Please, may be you can help me?

Alex:(

 yonchong September 10, 2012 17:45

It looks like the calculation is hitting the turbulence viscosity limit because the solution is diverging rather than converging.

There are a number of reasons why this could be happening but how are you initialization the solution? If you have the latest version try the hybrid initialization.

What does the velocity vector plot looks like? Is there any spike in the velocity plot?

 Alex_B September 11, 2012 01:42

Quote:
 Originally Posted by yonchong (Post 381112) It looks like the calculation is hitting the turbulence viscosity limit because the solution is diverging rather than converging. There are a number of reasons why this could be happening but how are you initialization the solution? If you have the latest version try the hybrid initialization. What does the velocity vector plot looks like? Is there any spike in the velocity plot?

I use hybrid initialisation.
I try to change mixture consistance (0.95 water + 0.05 air) and it's work and calculates well. I try to send printscreens of my initialisation.
Thank you !

 Alex_B September 11, 2012 03:34

5 Attachment(s)

 Alex_B September 11, 2012 03:36

5 Attachment(s)
continue of attachements

 Alex_B September 11, 2012 03:38

4 Attachment(s)
the last attachement)

 ghost82 September 11, 2012 03:39

Just a consideration, maybe it's not useful to you: have you set correctly primary and secondary phases?

For the first case: 0,95 air, 0,05 water air is the primary phase in the "phase panel";
For the second case: 0,95 water, 0,05 air, water is the primary phase.

Daniele

 Alex_B September 11, 2012 04:07

Quote:
 Originally Posted by ghost82 (Post 381165) Just a consideration, maybe it's not useful to you: have you set correctly primary and secondary phases? For the first case: 0,95 air, 0,05 water air is the primary phase in the "phase panel"; For the second case: 0,95 water, 0,05 air, water is the primary phase. Daniele

Yes, it is correct!
Thank you!

 Alex_B September 11, 2012 04:45

I seems to understand my problem!!!!!

So, I think that my mistake was big diameter of secondary phase.
Buy I try to check this.

 RodriguezFatz September 11, 2012 04:55

Hi Alex, some ideas:
1) Did you run a simulation with just air? Did it work?
2) Your grid is hard to see, but it looks kind of strange. Do all cells have the same size? Why wouldn't you have smaller cells at the walls?
3) Did you "patch" your zone to 5% water after initialization?
4) The other day, this message vanished after changing the inlet conditions. Did you try to set "Intensity and Hydraulic diameter" to somehow reasonable values?
5) What is the fraction of backflow of secondary phase at the oulet?

BTW: Your description / inital post is perfect. I wish everyone would introduce his/her problem like this!

 samidabest September 11, 2012 13:00

i'm new user on ansys ... and i have to work on ansys fluent so plz send me tutorials of ansys fluent 12 or 13 or 14 if any one have my email is samiullahh09me08.muet@gmail.com

 yonchong September 11, 2012 13:51

Open up Fluent and tutorials can be found in Help menu.

If not, just do google search on Fluent Tutorial. You will find plenty.

 Alex_B September 12, 2012 09:14

1 Attachment(s)
Quote:
 Originally Posted by RodriguezFatz (Post 381181) Hi Alex, some ideas: 1) Did you run a simulation with just air? Did it work? 2) Your grid is hard to see, but it looks kind of strange. Do all cells have the same size? Why wouldn't you have smaller cells at the walls? 3) Did you "patch" your zone to 5% water after initialization? 4) The other day, this message vanished after changing the inlet conditions. Did you try to set "Intensity and Hydraulic diameter" to somehow reasonable values? 5) What is the fraction of backflow of secondary phase at the oulet? BTW: Your description / inital post is perfect. I wish everyone would introduce his/her problem like this!
1) Yes, I tryed . It almost work (fluxes- ok, and velocity contours looks normal (I think)))))) (see attachement)
2) I have smaller size of cells close the wall.(mesn is ok)
3) Sorry, what mean ""patch" zone to 5%" ?
4)Where I can find "Intensity and Hydraulic diameter" parameters
5) fraction of backflow of secondary phase at the oulet- I havn't this parameter in outlet/ secondary phase/
I try to calculate the same task, but with symmetry conditions at the axis of me old geometry, and my calculation crushes(((

sorry, may be you send me your email, and I'll send you my case file? If it's ok for you (botyachkova.alexandra@gmail.com).

 RodriguezFatz September 12, 2012 09:33

3) When you initialize, Fluent sets the second phase density to zero inside your domain. You have to patch it "by hand" by clicking on the "Patch..." button just below the "Initialize" button. Here you can choose the domain and value you want to patch to a certain value! I guess the window will be self-explanatory. Setting the density fraction to, let's say, the inlet flow fraction will normally get the initial guess closer to the final solution.
4) You can find it in the inlet boundary condition panel under "Turbulence->Specification Method". You can choose between different ways of telling the solver boundary values for the turbulence - "Intensity and Hydraulic diameter" is one of them. You should also have a look at the turbulent viscosity by means of a contour plot. Where does the limitation problem occur?
5) Under "Boundary Conditions -> Your Outlet (2nd phase) -> Multiphase ->", can't you find a Backflow field? Try setting it to zero.

 Alex_B September 12, 2012 10:22

Quote:
 Originally Posted by RodriguezFatz (Post 381411) 3) When you initialize, Fluent sets the second phase density to zero inside your domain. You have to patch it "by hand" by clicking on the "Patch..." button just below the "Initialize" button. Here you can choose the domain and value you want to patch to a certain value! I guess the window will be self-explanatory. Setting the density fraction to, let's say, the inlet flow fraction will normally get the initial guess closer to the final solution. 4) You can find it in the inlet boundary condition panel under "Turbulence->Specification Method". You can choose between different ways of telling the solver boundary values for the turbulence - "Intensity and Hydraulic diameter" is one of them. You should also have a look at the turbulent viscosity by means of a contour plot. Where does the limitation problem occur? 5) Under "Boundary Conditions -> Your Outlet (2nd phase) -> Multiphase ->", can't you find a Backflow field? Try setting it to zero.

Thank you!
As I understand, you talk about Standart initialisation. But I use Hybrid.

 RodriguezFatz September 12, 2012 10:30

I am not sure, but I think it is the same for hybrid. Just click on initialize and than contoure-plot your secondary phase fraction. I guess it will be zero inside your domain. To initialize it with 0.05, you have to use the "Patch" button.

 samidabest September 12, 2012 13:17

i want to know to create the macros to use the macro model of heat exchanger in fluent

 All times are GMT -4. The time now is 07:48.