
[Sponsors] 
January 15, 2013, 23:11 
Drag force reduction in bus

#1 
New Member
Balaji
Join Date: Jan 2013
Posts: 6
Rep Power: 4 
Im doing a project in "Drag force reduction in bus".
I completed meshing using GAMBIT software. I did 2D and 3D analysis using FLUENT 6.3. I got the solution converged. I dont know how to read the "drag convergence" graph in order to find the Cd value. In 2D analysis i can able to see the pressure difference in front and rear side of the vehicle, but in 3D analysis i could not find the pressure difference between front and rear side of the vehicle. Also help me to find the Y plus value. Can anyone please help me????? 

January 16, 2013, 09:48 

#2 
Member
Yanlong Li
Join Date: Jan 2013
Location: BeiJing
Posts: 47
Rep Power: 4 
use DEFINE_ON_DEMOND marco


January 17, 2013, 07:05 

#3 
New Member
Balaji
Join Date: Jan 2013
Posts: 6
Rep Power: 4 
Hai " Yanlong Li " i couldnt understand what you have posted.


January 17, 2013, 08:25 

#4 
Member
Yanlong Li
Join Date: Jan 2013
Location: BeiJing
Posts: 47
Rep Power: 4 

January 17, 2013, 12:51 

#5 
New Member
Sárán Greene
Join Date: Nov 2012
Location: Dublin
Posts: 13
Rep Power: 4 
For your Y+ values you should be able to access them under "Plots  XY Plot" once here you tick the "Position on xaxis " box and make sure your x = 1, y = 0 and z = 0. Then move over to the "Y axis function" hit the drop down box and select "Turbulence". Directly under that box there should be another box. Hit the drop down menu until you find "Wall Y Plus" select it and hit plot. This should give you your Y+ graph.


January 17, 2013, 12:53 

#6 
New Member
Balaji
Join Date: Jan 2013
Posts: 6
Rep Power: 4 
Hai Yanlong Li,
Thanks for the reply. It contains lot of codes. What are the functions of those codes?? I dont know how to use that....In what way will it be useful for my project??? pls help me..... 

January 18, 2013, 00:11 

#7 
Member
Yanlong Li
Join Date: Jan 2013
Location: BeiJing
Posts: 47
Rep Power: 4 
Hi, BalaJi
I have three idears: 1. Use DEFINE_ON_DEMAND Macro to calculate every Cd and put it out; 2. Just use DEFINE_DPM_OUTPUT Macro to do it; 3. Use DEFINE_DPM_SCALAR_UPDATE Marco to calculate the Cd and creat an UDM to store it , I think this is a better way, cuz you can find this value in your postprocessing. see this Marco exapmle for detail. hope it can help you. 

January 18, 2013, 03:18 

#8 
New Member
Balaji
Join Date: Jan 2013
Posts: 6
Rep Power: 4 
Hai SARAN,
I got that graph. Thank you so much. 

January 20, 2013, 06:47 

#9 
New Member
Balaji
Join Date: Jan 2013
Posts: 6
Rep Power: 4 
Hai,
What is the significance of the Y PLUS value or what does it indicates ???? 

January 20, 2013, 12:49 

#10 
New Member
Sárán Greene
Join Date: Nov 2012
Location: Dublin
Posts: 13
Rep Power: 4 
In terms of boundary layer theory, y+ is simply a local thickness Reynolds number. In terms of CFD y+ is a nondimensional distance from the wall to the first grid point. In a practical sense, we don't resolve the solutions of turbulent flow by direct numercial simulation. This would require a very fine mesh near the wall in order to resolve the turbulent eddies in the boundary layer. Also, turbulence is time varying and random, so EVERY CFD model would need to be run as transient, even if the mean flow is steady state.
In order to deal with the temporal fluctuation of turbulence, we time average the governing equations. This is why you often hear CFD referred to as RANS (ReynoldsAveragedNavierStokes) analysis. But this is too good to be true. While on one hand we simplify the equations, on the other, the Reynolds averaging process introduces a new variable, so now we have a steady state problem with more unknowns than equations, and we all know that we can't solve a set of equations if we have more unknowns than we have knowns. So we need another equation(s) to close the Reynolds equations. The variable is known as the Reynolds Stress, and the closing equation(s) are known as turbulence models. Turbulence models deal with the flow in the boundary layer. The boundary layer is divided into an inner and outer region, and the inner region can be further subdivided into a laminar (viscous) sublayer and a fully turbulent region. For flow over a smooth flat plate with no adverse pressure gradients or other funky stuff going on, the inner region stretches from the wall out to about y+=150. The inner region is referred to as the "law of the wall zone" The fully turbulent part of the inner region is known as the "loglaw of the wall zone", and is characerized by a loglinear variation of the nondimensional velocity u+. In the viscous sublayer, it is assumed the u+=y+, and when plotted on loglinear graphs, it looks like the familiar Couette flow velocity profile that you see in an undergraduate fluids course. Now CFD codes assume that this viscous sublayer where u+=y+ happens between the wall and the first grid point. The first grid point is where code switches from the loglaw to the viscous sublayer. Generally this switch should occur at a value of y+ somewhere around 30. If your mesh is too fine near the wall, you will get a low value of y+. This will result in overprediction of the near wall velocity. On the other extreme, if y+ is too high, it will cause the code to apply the law of the wall to the outer wake where it is not valid. Okay, so I gave you a simplistic description. Things such as Reynolds number, surface roughness, adverse pressure gradient, etc will change the value of y+ where the velocity profile switches from the viscous sublayer to the log law of the wall. The value of y+ for the transition can range anywhere from about 10.8 up to 50. Further complicating matters is that some turbulence models employed by modern CFD codes can account for very low or high values of y+ and supposedly still give you reasonable accuracy. I hope that's all correct and is what you're looking for. 

January 29, 2013, 00:52 

#11 
New Member
Balaji
Join Date: Jan 2013
Posts: 6
Rep Power: 4 
Hai,
I am doing 2D analysis regarding "DRAG FORCE REDUCTION IN BUS". I have chosen "STANDARD KE model" as turbulence model. It had already crossed 4.5 lakhs iteration, but still i didnt get solution converged. It contains 4000 quadrilateral cells. Can anyone help me to fix the problem ????? I dont know where i made the mistake.... 

January 30, 2013, 18:02 

#12 
Member
Join Date: Sep 2012
Location: FL
Posts: 76
Rep Power: 5 
@tvn211
The KE model is most suitable for flows away from the wall. You can use it with wall function if you want to simulate the flow near the wall. You can do this only when you do not have high gradients of variables , separation or reattachment etc. You can go with K omega model. It does give proper results for flow near walls if you happen to resolve the boundary layer properly. @Saran1991 Most of it is right. But I think this part is not really true. "The first grid point is where code switches from the loglaw to the viscous sublayer. Generally this switch should occur at a value of y+ somewhere around 30. If your mesh is too fine near the wall, you will get a low value of y+. This will result in overprediction of the near wall velocity. On the other extreme, if y+ is too high, it will cause the code to apply the law of the wall to the outer wake where it is not valid." The first point ( non dimensionalized) is not the point where the separation takes place between the log law region and law of wall region. It is first point in the law of wall region. If you have flows near wall you need to have y+ values as low as possible (~1) so that it captures the boundary layer entirely. If you make y+ high , you not capture the entire boundary layer. That is the issue . CORRECT ME IF I AM WRONG. 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
ActuatorDiskExplicitForce in OF2.1. Help  be_inspired  OpenFOAM Programming & Development  8  July 3, 2014 10:54 
Too low drag coefficient on a bus  Roland R  CFX  8  September 21, 2012 05:23 
Force can not converge  colopolo  CFX  13  October 4, 2011 22:03 
Force vectors for drag during sweeping motion  aamer  FLUENT  0  April 18, 2011 08:17 
formula used for drag force?  kamma  Main CFD Forum  0  April 2, 2010 10:21 