
[Sponsors] 
June 14, 2008, 05:33 
Directional Loss Model

#1 
Guest
Posts: n/a

I'm doing a case of SCR(Seletive Catalytic Reduction, a DeNOx device applied in power plants) reactor now. The Catalytic Layer is located in the Reactor, and I want to use the Directional Loss Model to simulate the pressure drop across the layer. Though there is a case("Flow in a Catalytic Converter") in the CFX Tutorials, but an important difference is that in my case I don't know the exact "resistance coefficient"(Kq), while in the Tutorial case a value of 650 [kg m^4] has been directly given. However, what I know is the design parameter of the "Pressure Drop" across the layer(DeltaP = 435[Pa]) and the "Catalytic Layer Height" (DeltaH = 11.4 [m]). According to the equation stated in the Tutorial, I've simplified it into: DeltaP/DeltaH = Kq * abs(U)*Ui I defined a CEL expression to represent the Kq value, which goes like this, Kq = DeltaP/(DeltaH * sqrt(Velocity u * Velocity u + Velocity v * Velocity v + Velocity w * Velocity w) * Velocity v ) After running it in CFXsolver, the "Fatal Overflow" error occurred unexpectedly, since I've ever tried to directly set a Kq value, say 100 [kg*m^4], it can complete normally. I dont know how come it happened. If you have any idea about how to solve this problem, plz let me know! If you are interested in my case, personal contact through Email (wateraction@126.com) or MSN (wateraction@hotmail.com) is encouraged. Thanks very much for your attention!


June 24, 2008, 11:46 
Re: Directional Loss Model

#2 
Guest
Posts: n/a

If Velocity v is zero (usually the initial guess for the velocity data field) your expression will turn to DeltaP/(DeltaH*0), thus division by zero. This might your problem with the "Fatal Overflow".
You have to make sure, that [ sqrt(Velocity u * Velocity u + Velocity v * Velocity v + Velocity w * Velocity w) * Velocity v ] doesn't evaluate to zero. You could try to check for zero velocities and "replace" it with a sufficiently small velocity in your Kq expression, like: Kq = DeltaP/(DeltaH * ( Velocity * Velocity v + step((Velocity*Velocity v)/1[m^2 s^2])*step((Velocity*Velocity v)/1[m^2 s^2])*1e10[m s^1])) 

June 25, 2008, 01:48 
Re: Directional Loss Model

#3 
Guest
Posts: n/a

Thank you very much, hsr, but can you tell me what does step mean?


June 25, 2008, 02:16 
Re: Directional Loss Model

#4 
Guest
Posts: n/a

step(<var>) checks whether <var> is
: 0 returns 1 = 0 returns 0.5 < 0 returns 0 <var> must be dimensionless, that's why you have to divide the velocities by 1 [m s^1] so when you evaluate step(<var>)*step((<var>)) it will return 0 for var > 0 and 0.25 for var = 0. It would be nice to use something like "if (<var> > 0) then", but for this you'll have to wait until CFX 12 is released or use user fortran. 

June 26, 2008, 12:38 
Re: Directional Loss Model

#5 
Guest
Posts: n/a

Thanks for your explaination，hsr, I've learned a lot. I agree with you that using "if" sentence would be nice since it's simple and easy to understand. While for the Fortran language, I've never learned it though people say it's not hard to get on hand. Really expecting the 12.0 version coming soon.


Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
help for different between les model (subgridscale model)  liuyuxuan  FLUENT  1  October 2, 2009 15:25 
Grid resolution for fullscale and down scaled model  gravis  Main CFD Forum  0  October 2, 2009 10:27 
LES and combustion model  Margherita Cadorin  CFX  0  October 29, 2008 06:24 
Directional loss model  Claudia  CFX  3  February 8, 2007 21:15 
KatoLaunder model  sam  Main CFD Forum  13  September 21, 2006 10:15 