Drag Coefficient Flow over a Block
 

Dear Community,

I am trying to simulate a simple model for verifying the drag coefficient from crosswind. It is a block inside a wind tunnel.

I am trying to mimic the results from other paper which get the value of drag coefficient of 1.4 from CFD and wind tunnel experiment. However, I tried so many simulations in starccm+ v 9.04 but only getting Cd around 1.18.

I have been working on this for more than a month and really need some advice for getting similar value to the paper.

The boundary condition I used is
1. Inlet, (velocity inlet for constant density and stagnation inlet for Ideal gas)
2. Outlet
3. Symmetry walls for wind tunnel walls (wall parallel to the flow)
4. Non-Slip for Ground and the Block

I am using k-e turb model with Re = 160,000
My y+ value is less than 1 for the Block.

I know it is a very simple problem but I can't nail this problem down.
I really appreciate the help !!

Are you using the same physics setup that they used in the paper? They probably document that.

Also try easing up on your y+ values. I was told by cd-adapco guys that for k-e with all y+ wall treatment to target between 1 and 5 or 30 and 60 for best results.

There is also the chance that you aren't normalizing your coefficients to the same area.

Also, have you done a mesh dependency study? It could be that your mesh isn't refined enough.

I did mesh study. I got 800k, 3M and 11M mesh for the case.
I also set up the geometry of the vehicle and the wind tunnel to be the same as the paper. I dont know how to attach paper in this forum.

Can you post some images of your mesh?

Also is your simulation steady-state? What does the drag convergence look like?

I am not so sure of the k-e model. In my experience, the k-w sst model worked well for aerodynamics. You could give that a try.

Also, I would not use symmetry for the wind tunnel walls.

k-e is the model recommended by CD-Adapco for most external aero problems. k-w can be unsteady in some situations, but k-w/sst has been shown to capture certain phenomena better. I would say that if the paper uses k-e, stick with k-e otherwise you aren't comparing apples to apples anyl onger.

Dear All, thanks for the respond.

I am running steady state condition. the Cd is oscillating in a range if I use couple solver and very steady when I use segregated solver.

Are this images clear ?

http://oi58.tinypic.com/sy7bb8.jpg
http://oi59.tinypic.com/2j14jgm.jpg

When you type a message there are icons above the text box. If you hover your curssor over them they will display their function. One of them looks like a paper clip, that can be used to attach images. However, they limit file size and it sometimes be a challenge to compress images small enough.

As for your oscillating drag coefficient, that is totally normal. You have a blunt body that is experiencing vortex shedding. The drag coefficient is oscillating with the wake.

http://en.wikipedia.org/wiki/K%C3%A1..._vortex_street

Honestly, if you are seeing a significant amout of oscillation you shouldn't be doing a steady state analysis. The term steady is a little misleading here as the solver still uses a psedo-time-step to advance the solution and will still show unsteady behavior. You can't force a steady solution where one doesn't exist.

That being said, all you have to do to get your true drag coefficeint from a plot of the oscillation is right click on the plot in the design tree and select 'tabulate'. This will create a table you can copy into a spreadsheet. Then you just need to average over several oscillations (taking care to capture full periods of the oscillation).

Work though the Solution Recording and Playback: Vortex Shedding tutorial. It should be very similar to what you are doing.

Sorry, I didn't see the bit about segregated solver. Coupled is a more robust solution and generally more accurate (all things being equal). Segregated will save you some time, but its a little rough around the edges. I prefer to do coupled analysis whenever I can. That's just my personal preference though.

http://oi57.tinypic.com/nozplw.jpg

This is my Cd Plot. This the current result I got and Cd is about 1.0.
It looks converged after 5000 iterations.
Im using couple solver, k-e for this run with stagnation inlet.

I cannot access that web site. Try attaching the image like I explained, not inserting one from the web.

Apologize. I updated the attached pictures with insert option.

Much better. On your force coefficient plot, can you change the x axis to show only iteration 2000 to 5000 and the y axis to show +/-2. Your startup oscillaitons are so large that it makes it hard to see what you are interested in.

You also can probably cut your run time in half by using grid sequencing initilization (under solvers > coupled implicit > expert initilization. The default settings should be good for your case.

I updated the Cd plot above

That looks fairly normal. However, since you don't have a true sinusoidal oscillation you will have to just average over a long span. Take several different averages, each with a different span and compare them to make sure your selection isn't affecting your average.

As for why your not getting the correct magnitude, it could be lots of things.

1. Did you ever veryify that your reference areas are the same between your calc and the report?

2. Did they use the same type of mesh?

3. Try loosening your mesh your mesh and targeting 1<y+<5.

4. Try adding more wake refinement.

5. Try the k-w model too. It never hurts to try and it could bump up your Cd a bit.

6. Can you post a link to the paper so I can see what your are trying to do?

1. What do you mean by the area reference? I calculated base on the frontal area of the vehicle which is the width and the height of the block.
2. They use much coarser mesh and using LES turbulent model.
3. I will try this. I thought its the best to keep y+ bellow 1.
4. I did refined my wake mesh before and the result didn't change much (less than 1% difference)
5. I also did the k-w run. The result from it has more oscillation and yes it bump my Cd by 0.05 to 0.1.
6. The Link of the paper (I can email you the paper). I am trying to reproduce their simulation for non-moving block without the windbreak.

Journal of Wind Engineering and Industrial Aerodynamics, Volume 116, May 2013, Pages 61–69.
"Windbreak protection for road vehicles against crosswind" by Chia-Ren Chu et. al.
http://www.sciencedirect.com/science...67610513000500

His Thesis is free to download.
( https://www.google.com/url?sa=t&rct=...,d.eXY&cad=rja)

When you normalize a force into a coefficient you typically do it like this:


Cd = Drag / (dynamic pressure * Area)


The area is totall arbitrary, it sounds like you made a logical choice. All I am saying is you should make sure you use the same area that the do in the paper. Obviously, having a different denomenator will give you a different Cd for a given drag.


If they did a LES simulation, why would you try to compare it to your k-e simulation? They are radically different in nature and require very diffent mesh considerations. It's also strange that you are doing a RANS simulaiton with higher mesh resolution than an LES analysis. LES requires VERY fine grid and small time step sizes. RANS uses caluclated averages for the turbulene fluctuations over your much larger time step.

The y+ requirement is heavily dependednt upon your turbulence model, and as I said for k-e with all y+ wall treatment you shound stay between 1 and 5 or 30 and 60. That being said, your mesh is way too fine for your current approach. If you want to compare, do EXACTLY what the paper did. Work tutorials, read the help manual, and if you have access try talking to tech support. They are very helpful.

I will try to take a look at the paper later, but it sounds like your issues stem from a lack of understanding of the models you are applying.

I understand that I am not following the model that they are using and also questioning their mesh resolution. However, what I really want to replicate is the experimental result. I was thinking that even though I am using RANS, I should get Cd close to 1.4 instead 1.18.

My final goal is to simulate a simple block for modeling a crosswind for verification purpose. I believe that I should get the Cd value about 1.4 from most paper I read.

I already tried to run starccm for a road sign structure and I got a good Cd agreement from the experimental data. But the flow is not influence by ground effect.

From most papers, for crosswind problem, their Cd value range is about 1.38 - 1.45.

No matter how I set up this block case, with different turbulent model, incompressible or compressible. My Cd value always range is 1.15 to 1.23.

Do you have any advice how to simulate this case, a flow over a block for crosswind problem?