CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   Drag force reduction in bus (http://www.cfd-online.com/Forums/fluent/111807-drag-force-reduction-bus.html)

tvn211 January 15, 2013 23:11

Drag force reduction in bus
 
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?????

Yanlong Li January 16, 2013 09:48

use DEFINE_ON_DEMOND marco

tvn211 January 17, 2013 07:05

Hai " Yanlong Li " i couldnt understand what you have posted.

Yanlong Li January 17, 2013 08:25

Hi,
You can see this website:
http://www.cfd-online.com/Forums/flu...particles.html

Saran1991 January 17, 2013 12:51

For your Y+ values you should be able to access them under "Plots - XY Plot" once here you tick the "Position on x-axis " 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.

tvn211 January 17, 2013 12:53

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.....

Yanlong Li January 18, 2013 00:11

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.

tvn211 January 18, 2013 03:18

Hai SARAN,

I got that graph. Thank you so much.

tvn211 January 20, 2013 06:47

Hai,

What is the significance of the Y PLUS value or what does it indicates ????

Saran1991 January 20, 2013 12:49

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 (Reynolds-Averaged-Navier-Stokes) 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 "log-law of the wall zone", and is characerized by a log-linear variation of the nondimensional velocity u+. In the viscous sublayer, it is assumed the u+=y+, and when plotted on log-linear 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 log-law 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.

tvn211 January 29, 2013 00:52

Hai,

I am doing 2D analysis regarding "DRAG FORCE REDUCTION IN BUS". I have chosen "STANDARD K-E 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....

victoryv January 30, 2013 18:02

@tvn211

The K-E 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 log-law 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.


All times are GMT -4. The time now is 00:09.