Guys, I really need help here. Currently I am doing my final year project with the help of FLUENT. I am trying to study the drag coefficient for flow around a cylinder with Reynolds number varies from 10000 to 10000000. Unfortunately, I could not get the proper result. The result I get is different with the result shown in book. I checked every step I did and there's nothing wrong with that. Here are the steps I did to get my drag coefficient.

I go to REPORT, then I choose FORCE and FLUENT prints the value for total force, which is the sum of pressure force and viscous force. I take the total force and apply it into the drag coefficient formula, which is Cd = 2F/(density*area*velocity*velocity).

Is there any problem with my step?

Thanks.

hey i am not sure but take a look at reference values

i suffered same but in some other context

Use the reference values to calculate the Drag force coefficient for you. You can either manually enter the reference density and velocity, or you can tell it to calculate these from a boundary (like your inlet bc... this is the method I recommend).

Also, are you working in 2D or 3D? If you're working in 2D, be careful of the "depth" in the reference values. This is the length going into/out-of the view plane (it's the Z-Coordinate). The value defaults to 1m, which is good if you're working in meters and you're looking for "Newtons per meter", but will throw your calculations off if you're working in any other length scale/units.

Beyond that, start checking your solution. Is your mesh refined enough, are your boundary conditions properly applied (are you getting the density/velocity you expected), etc...

Post a note to let us know how this is going.

Hope this helps, and good luck, Jason

I am working on 2D problem. I try to match my result with the result shown in textbook. But the result from textbook, they do not specified the value for depth( the length in Z direction) and they manage to get the drag coefficient. I wonder why?? Here's the link http://www.princeton.edu/~asmits/Bicycle_web/blunt.html I try to match with the Cd for circle in figure 1 with Re=10 to the power to 7.

I tried with the reference value and calculate from my BC, and error occur(floating point error, divide by zero) when i go to report and try to print my drag coefficient, pressure force etc. Then i try to set the reference value by myself and get close result but not accurate enough. ish....

Because they used a unit length. Typically your drag coefficient equation is:

Cd = F / (0.5*rho*V^2*A)

Your reference area is A=D*L, but if L = 1, then A=D. Therefore when using a unit length, you get:

Cd = F / (0.5*rho*V^2*D)

Be careful of the units, always defaults to 1m. So, if you're working in feet, then the default depth is still 1meter (~3.28ft).

The divide by zero sounds like there might be a problem in the setup. Something is being set to zero that shouldn't be. When you calculate from your BC, what reference values are calculated (do they match what you expected for Velocity and Density?). This could imply a problem with your boundary conditions. If you check your boundary conditions (either using the report tools or the plot tools) are you getting the conditions you expected?

Jason

The flow around a cylinder is unsteady (vortex-shedding), three-dimensional and turbulent.

If you carry out 2D steady simulations, maybe the best turbulence model is k-w SST. For Re=10000 the boundary layer is still laminar, so you should use the low-Re formulation (tick the "transitional model" in the k-w menu). For higher Re numbers, with turbulent boundary layer, you should retain the low-Re formulation and use a mesh fine enough to solve the viscous sublayer. Maybe with this combination you will succeed in getting better results in comparison with experimental data.

If you carry out unsteady simulations, you should use k-w SST DES model, but probably you are going to overpredict the drag due to the lack of 3D effects in the wake. Other problem is that you must check for the console instruction to allow fluent to use DES in 2D simulations (using the standard menus, fluent only allows les and des simulations for 3D problems). I am not sure but for 2d les or des you should type (rpsetvar 'les-2d? #t) in the fluent console.

Other reason for not getting the right values of drag coefficient may be related for the convective interpolation. For recirculating flows, forget the standard first-order upwind scheme. Use at least second-order upwind scheme in your simulations.

I did and tried all the possibilities and guides from you all but still cannot. The results do not match! How~~~

Fabio's right about the turbulence models. Your best option is the k-omega with transitional correction applied. This requires y+ of around 1. So you need a properly defined mesh (you're probably going to need meshes for each condition, and it'll probably take a couple tries to get the mesh right for each condition). I'm not sure how good this model is at really capturing the transition point though. Probably not great (but I don't have any evidence either way to confirm that)... starting at the low end, I'd also carry a laminar solution along for each condition and see how either solution compares with the results, and how they compare with one another (especially at the low Reynolds numbers).

Other problems could be your boundary conditions, your material selections, your solver, etc. Tell us more about what you've done for a setup. Also, when you look at a solution, look at the dependent variables and see how they compare to what you'd expect (if you use a pressure inlet, look at the static pressure and velocity... if you use a velocity inlet, look at the pressures...). This could point you to problems with your BCs.

Also, the part where you get a "divide-by-zero" error when you calculate your reference values from your boundary condition doesn't sound right. What were you expecting for reference values, and what did it give you?

Thanks, Jason

I guess the problem appears due to my meshing. Any guide on how to mesh a rectangle with a hole at the middle? This is a 2D problem. First, I build a rectangle (face) and the I build another circle(face) at the middle. After that i subtract the circle from the rectangle. After that I could not make a proper mesh. Any idea please? The meshing from Quad-Pave does not seems very good. Any other ideas?

Separation is typically difficult to predict. Including a boundary layer mesh will help, but since the geometry is pretty simple, I recommend using a structured mesh. I feel it gives me better control of the mesh. I still recommend using the boundary layer mesh tool, it will help you with the near wall mesh, but outside of that you can't control the mesh growth very well (I know, some people will point out sizing functions, but with a structured mesh, I find it easier, faster, and more predictable to just control the mesh myself using edge gradients).

For an example on how to decompose the domain, check out: http://www.ansys.com/products/flowla...r_tutorial.pdf

This was done using Flowlab, not Gambit, but it shows you a pretty good breakdown of the flowfield, and a rough idea of what your grid should look like... but your first layer may need to be more or less refined (and always smoothly grow from your smallest layer! that's where the boundary layer mesh can be helpful... works great in simple geometry... not so well in 3D, and doesn't work at all for complex 3D geometry)... estimate your y+ with one of the online calculators, then check it in Fluent and adjust accordingly.

For an example using edge gradients in Gambit, check out: http://courses.cit.cornell.edu/fluent/pipe2/step2.htm

Some other good tutorials, examples, intro information available through Cornell: http://courses.cit.cornell.edu/fluent/index.htm

Hope this helps, and good luck, Jason

Guys, I guess my problem is due to the improper meshing on gambit. These are the steps that I did previously. This is a 2D problem. First, i build a rectangle(face) and then I build another circle(face) at the center of the rectangle. After that i subtract the circle from the rectangle and finally i get a rectangle with a hole at its center. Then, I could not get a nice and proper mesh. I tried with Qua/Pave but the meshing is not good enough. Any other guide on how to do the meshing for this simple geometry????