CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CD-adapco (http://www.cfd-online.com/Forums/cd-adapco/)
-   -   WARNING #090 (http://www.cfd-online.com/Forums/cd-adapco/55269-warning-090-a.html)

echo April 1, 2006 22:23

WARNING #090
 
Hi,everone i'm doing a catalyst converter simulation, adopt the k-Epsilon/high Renolds Number,and define the inlet and outlet boudary. But when i run ,i encouter this warning:***WARING #090 *** VALUE ELOG*YPLUS OR ELOG *EFFVIS/(CAPPA*VISCOS) IS LESS THAN 1.1 AT 3334 CELL.UPLUS=YPLUS LAW IS USED. IF THIS SITUATION PERSISTS,INCORRECT RESULT MAY BE OBTAINED. what does this warning mean? How should i sovle it? Thanks for answering. i have done the search on this forum,but i can't read the message before this year.Thanks again


Ben April 2, 2006 07:15

Re: WARNING #090
 
It means your yplus is low in 3334 cells, if this is a lot of your model or it persists throughout the simulation you will need to consider changing the mesh or the turbulence model. If it is a very small part of your model or goes then just ignore it.

echo April 2, 2006 09:28

Re: WARNING #090
 
This warning appears at the first. So should i change the model? then how should i change it? And the run can't converge also, does the warning result this?thaks again

Ben April 3, 2006 06:34

Re: WARNING #090
 
Does the warning go away or the number of cells it is called for reduce significantly? Also is this a transient or SS run?

echo April 3, 2006 08:24

Re: WARNING #090
 
Sorry,i don't know the SS. What is it mean? I do a steady, uncompressible turbulent flow simulation in a catalyst converter. The warning goes through the whole analysis process and there is always and just a cell having this warning every iteration. And the run can't converge too. Thanks!

Kalle April 3, 2006 13:20

Re: WARNING #090
 
Activate a low Re model and use hybrid wall functions (and the error will go away)

ben April 3, 2006 15:13

Re: WARNING #090
 
Although it may not converge the simulation, SS stands for steady state by the way. What is the convergence like and which residual is the worse?

echo April 4, 2006 09:24

Re: WARNING #090
 
When I run the analysis under the windows in starcd 3.22, there will not run for one iteration and diverge. But I run the same model under linux in starcd 3.26 ,there will run 133 times ,and the mass is worse. Why should this situation happen?thanks!

echo April 4, 2006 09:51

Re: WARNING #090
 
I try it just as you told, there isn't the warning now. In this model, Re=141138 and the v=53m/s. Shouldn't I use the high Re medel? And the run can't converge too. It runs no time.thanks a lot!Wishing your guide!

Ralphie April 5, 2006 05:01

Re: WARNING #090
 
You should read at least some of the documentation that comes with Star-CD. The difference between the High-Re and Low-Re turbulence models is not that one is used for large Reynolds numbers and the the other for small ones. The difference is in the wall treatment. You need different mesh densities near the wall for each model.

Divergence can be caused by numerous reasons: Insufficient mesh quality, transient behaviour, unsuitable physical models/properties, etc... You can try reducing the relaxation factors for a start.

echo April 5, 2006 06:23

Re: WARNING #090
 
Thanks for your guide!I have try reducing the relaxation factors and increasing the number of sweeps of velocity.I also reduce the relaxation factors of pressure.But these have no effect too.I have tried the catalyst model of the tutorial of proam and imposed the condition of steady state and High-Re turbulence model and standard wall function, defined the inlet and outlet boudary. It diverge also and have the warning. I really don't know what I should do!

Ben April 5, 2006 08:22

Re: WARNING #090
 
go on the basic training course!

echo April 5, 2006 08:34

Re: WARNING #090
 
OK!I'll try! Thank you! But do you have other guide?

Ralphie April 5, 2006 09:35

Re: WARNING #090
 
Are you sure that your mesh is ok? did you check the results you are getting? do they look plausible? Are you using anything like porosity, energy calculation, chemical reaction etc? is there a possibility for unsteady behaviour of your flow?

echo April 5, 2006 09:40

Re: WARNING #090
 
Yes,I use the porosity.I have check everthing ang there is no problem.I think the mesh is ok.Does the porosity influnce this? Thank you!

Ralphie April 5, 2006 10:00

Re: WARNING #090
 
Try and switch the porosity off and start again. Where do the values for alpha and beta come from? Do they make sense? What kind of mesh do you use? How many boundary layer cells do you have?

echo April 5, 2006 21:13

Re: WARNING #090
 
It converge when i switch the porosity off. Does the alpha and beta influnce this? I just calculate them from the equation dp/dl=-a*v2-beta*v from others experiment. Do they just get from this method? And I don't know if the experiment is right. I just find the experiment in the paper. And I use the tetrahedral mesh produced in the praom. There are 293075 cells in all and 42588 boudary layer cells and three layers. Thank you a lot!

echo April 9, 2006 20:40

Re: WARNING #090
 
Hi,Ralphie I have changed the mesh of the medel and it converge now. Thus does the mesh precision influnce the convergence?

Ralphie April 10, 2006 06:58

Re: WARNING #090
 
It most certainly does!!! It is not just the precision but the quality of your cells. There are quite a few tools in Star-CD that help you to find your bad quality cells. Furthermore there are certain guidelines on how your wall boundary layer has to look like. Read the manuals and some CFD literature too. Good luck with the next project!


echo April 11, 2006 06:22

Thanks foy all your attention and reply *NM*
 


All times are GMT -4. The time now is 17:47.