hi..

please help me in getting the Cd value for flow past a circular cylinder....

diameter = 2m

medium = water

i checked with segregated solver unsteady flow and for Re = 10^4 i'm getting Cd in the range of 0.01. but standard results say the Cd value shud be around 1.2 .what is the problem?? how to set the REFERENCE VALUES????

since i'm using water, viscosity is 0.001003 and density is 1000.so the flow velocity becomes very less to get the required Re. also please tell me the area to be calculated... i mean

Cd = D/(1/2 *rho*v^2*A)

the area A is the frontal projected area....for circular cylinder normal to the flow..how to calculate the area???? is it (pi*d^2)/4 or (d*1) since drag per unit length or something else....

in REFERENCE VALUES there is an option called 'depth' and 'length'....what shud be the values...i'm getting very less values of Cd... for Re = 10^6 i'm getting around 1 . but i shud get around 0.5 ...please help me with ur suggestions...

THANKS IN ADVANCE...

ANY HELP IS HIGHLY APPRECIATED.... REGARDS karthik

you have to divide by d*l (i.e if you are using periodic b.c. in the spanwise direction). Also in the reference values check to make sure the reference velocity is what you give at the inlet. else you have to divide by v^2. Your reference denisty and viscosity should be the values for water that you indicated. In FLUENT those values are taken by default. But check to make sure.

Length is the reference length used in moment coefficients (Cm = M/(1/2*rho*v^2*A*L)

Since you have depth listed in your reference values, it means you're running a 2D simulation. Depth is the measurement in the third dimension... or how far into the screen your model goes. Lets say your cylinder is only .25m long... then use .25m as your length. If you want to get numbers per unit length, then put one in for the depth.

As far as calculating the area... for a 2D cylinder, I typically see the reference area as pi/4*D^2 and the depth is taken as per unit length, and for a 3D cylinder I've seen it both ways (pi/4*D^2 or D*depth).

Good luck, Jason

hi

thanks for ur useful info....actually since its a 2D case....the cylinder is infinitely long.....and i'm getting reasonably acceptable values if the medium is AIR. when i change the medium to WATER, i'm getting very less values (in the range of 0.01 instead of 1.2 which is the actual Cd value for a circular cylinder with Re in the range of 10^4 or 10^5)....but the medium has got nothing to do with the Cd since it is Re number dependent....thats why i'm getting confused.....

shud i increase the domain....will that help me in any way...

has anyone performed this sort of Cd calculations with water as medium....

please put in ur suggestions.... thanks to Ben and Jason....

thanks in advance to others....

regards

karthik

hi sorry i forgot to say one thing....i put depth value as 1 since to get drag per unit lenght and also since its an infinitely long cylinder....

but when i increased the value of DEPTH i cud see Cd value going up......

what to do now??

karthik,

In this case, depth should be 1 because predicting Cd and Cl over a circular cylinder is a 2D problem. Do not worry about depth.

I think your main problem is the area. You should set the area according to the flow direction. Therefore, the area here should be the diameter of the cylinder not pi*R^2. Set the velocity and density as what you define. This should solve your problem.

If you have any other question, feel free to e mail me as I am simulating similar situation.

Sham.

hi what sham mentioned is correct use diameter for area & depth as "one " and length as " your cylinder diameter" for your 2d case and,if you are changing the medium to water in boundary condition panel (not in materials panel) go to fluid and check whether the water is choosen there or still the default air is highlighted if air then change to water then only yo will get the water viscosity and density in reference pannel don't take this as advice, please avoid using " TWO D" simulation for such a high (subcritical) reynolds number.if you are simulating 10000 reynolds number in two D flow and getting the exact result means that what the physics behind the turbulence is meaningless.

I thing yuou will get everything fine bye Ayyappan.T

hi

thanks ayyappan....and thanks other too....i have got the results...ayyappan, as u told...the mistake was in the fluid option in the boundary condition.... yesterday only i checked it and changed it...now i'm getting reasonably correct answer....

i'll do for turbulent case too.... thanks a lot friends....

regards

karthik