i have problems calculating coefficeint of drag using fluent; for the flow over cylinder (L/d = 10) ,Mach no.= 1.3 i am solving in 2-D

The flow field seems to be ok , but the problem is with the "refference values" i set for the calculation of coefficients. I have given the frontal area according to the problem and the values such as velocity and rho is of free stream.

The Question is:

How does i get to know the right valvue for the "Depth"? (as it changes the coefficient drastically). "Length" on the other hand does not have an influence. Fluent manuall also does not say much about it.

I am solving in 2-D with L/d = 10 and length of the cylinder parellel to the flow direction.

What will we set the "Depth" in "Refference Values" and why ?

Depth is your third dimension. It's how far into the screen your 2D model goes. The force coefficients are: Cf=F/(1/2*rho*V^2*Aref) (where F=the calculated force, rho=the density in your reference values, V=the velocity in your reference values, and Aref=the reference area) To calculate the force (F), it calculates the force/unit length on the 2D section, then multiplies it by the length you specify as the Depth (which is why it changes your force coefficient). The reference length comes into play when calculating moment coefficients: Cm=M/(1/2*rho*V^2*Aref*Lref) (which is why it doesn't change your force coefficients) For a cylinder PERPENDICULAR to the flow, Aref=pi/4*D^2, Lref=D, and Depth=D*(L/d) (where you stated your L/d is 10).

For a cylinder PARALLEL to the flow, then a you would go with a 2D axisymmetric case. The depth isn't used in this case. Fluent calculates the forces based on a 2*pi rotation. Make sure you select it as an axisymmetric case, otherwise Fluent sees your model as a straight extrusion (which makes your model a block with the depth you specify in the reference values, not a cylinder).

Hope this helps, Jason

Thanx its great help.

Cd is now comming fairly reasonable.

can you please elaborate on solving the 2-D case as axisymmetric case in fluent, may be this will improve the results even better.

Thank you again for such valuable help

bye

Well what do you want to know?

I'll throw some info out there...

2D Axisymmetric cases are for bodies of revolution (take a profile and spin it 360° around an axis, like a bullet, a vase, etc...). Quick example why you would run an axisymmetric model: the angle of the oblique shock coming off the front tip of a wedge is different than the angle of the oblique shock coming of the tip of a cone, even if they have the same angle of incidence.

If you're running a case where the AXIS OF REVOLUTION IS PARRALLEL TO THE FLOW then you should run an axisymmetric model, not a normal 2D model. You can turn on the axisymmetric model by running fluent 2d, and then Define->Models->Solver, and you'll see an option under Space for Axisymmetric. Be careful when modeling this... your axis of revolution MUST be on the x-axis, and your entire mesh must be above the x-axis. You can translate the mesh if you have to in FLUENT (Grid->Translate), but you can't flip it. That seems to be the most common problem with axisymmetric modeling.

Hope this helps.

Goodluck, Jason

Thanx jason, i will try this out immediately.

jehanzeb

hi

the problem is that the solution diverges. i have tried all the turbulence models. the same case when solved in simple 2-D case the solution converges well with all the turbulence models.

goemetery starts at (0,0) and is above x-axis (the axis of revolution)

any help would be appreciated

Ok... Did you change the boundary condition to axis (I forgot to mention that before... you have to change the boundary that is the axis of revolution to an "axis" boundary condition)?

If so... what are you using for a solver (segregated, coupled implicit, coupled explicit), and what are you using for solver settings (under-relaxation factors, discretization settings, and courant number(if using the coupled solvers))? Can you list what you're using for boundary conditions as well as your operating conditions?

Thanks, Jason

hi

well i got convergence with improving the grid. But i think the solution is not realistic.

let me tell u first the parametrs i am using.

yes i changed to the axis boundary condition.

Coupled , implicit, 2-d Axisymmetric, underrelaxation factors are 0.25 for all. Courant no was kept 1 initially but later changed it to 5 . Discretisation schemes used were 2nd oder upwind schemes for all. Viscous models used was k-epslon (standard) initially but later changed to SA as solution got some initial kick.

Cd (coefficeint of drag) is comming reasonable , (0.3) countours are also some what reasonable(not as good as that for 2-D case),flow disturbance is minimal in this case and Oblique shock wave is closer in this case as compared to the 2-D case.

but the problem is with the STREAM FUNCTIONS.

Stream function dont intersect, thats ok. But they are seperated (dont pass close to the object) away from the Object (The Cone) ie they have no influence of the object i think.

i have also tried to make finer mesh, but is doesnt work out.

another thing i have value of of Y+ of oder of 1e+3 on the surface, is it ok.

thanx

jehanzeb

For the k-epsilon model, I believe that you want a y+ value between 3 and 300. I've heard of having y+ as high as 2000, but I don't know how valid it is, or what kind of pit-falls you might be running into.

Where are you getting your stream function? Do you mean you're plotting pathlines and they are not coming close to the object? The oblique shock is going to do most of the work of turning the flow. If your pathline starts too far from the axis of symmetry, then the shock will turn it away from the object. If you look at the vector plots, this will give you a better view of the flow directions close to the body.

Another thing to check is the gradients (Adapt->Gradient). Since you're using the coupled solver, you'll probably want to adapt by density.

Goodluck, Jason

hi no i am talking about the STREAM FUNCTIONS(stream lines) not the path lines ie. Contours---> Velocity--->Stream Function (Filled Option unchecked).

the streams function dont pass close to the object. in actual they should pass close to the object. may be this is due to axisymmetry BC i am using. ( any comment? )

Velocity Vectors are fine.and about Grid Adaption , i tried but there were no cells marked for refinement.

Thanks a lot!

jehanzeb

Can you e-mail me an image of what you're talking about? jason_at_bae@yahoo.com

I have a feeling that the solution is valid... try changine the range (turn off auto range and then set a smaller value for the maximum) so that you're getting better resolution near the axis of symmetry, which is where the flow is coming from that is going to be close to the body.

Thanks, Jason

Hi Jason

That did the trick. the countours are fine now. i also had the feeling that the solution was correct, but was not 100% uptill now.

And how could i thank you for such great help you have been. Good Luck in any thing you do and a Bundle of Thanks.

Jehanzeb