# drag co-efficient for circular cylinders

 Register Blogs Members List Search Today's Posts Mark Forums Read

 August 16, 2005, 01:13 Re: drag co-efficient for circular cylinders #2 Ben Guest   Posts: n/a 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.

 August 16, 2005, 08:25 Re: drag co-efficient for circular cylinders #3 Jason Guest   Posts: n/a 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

 August 16, 2005, 09:10 Re: drag co-efficient for circular cylinders #4 karthik Guest   Posts: n/a 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

 August 16, 2005, 09:13 Re: drag co-efficient for circular cylinders #5 karthik Guest   Posts: n/a 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??

 August 16, 2005, 09:19 Re: drag co-efficient for circular cylinders #6 Sham Guest   Posts: n/a 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.

 August 16, 2005, 12:25 Re: drag co-efficient for circular cylinders #7 ayyappan Guest   Posts: n/a 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

 August 17, 2005, 02:25 Re: drag co-efficient for circular cylinders #8 karthik Guest   Posts: n/a 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

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Cheng CFX 8 May 4, 2017 17:48 kamma Main CFD Forum 0 April 2, 2010 10:21 Romain FLUENT 0 February 28, 2006 19:35 jehanzeb FLUENT 11 December 27, 2004 02:41 Axel Rohde Main CFD Forum 1 November 19, 2001 13:19