help
 

Hello,

At first I use around 50000 cells but the results I get is around 50% lower than the experimental values. I was thinking that the mesh is not fine enough. Then I increase the mesh to around 100 000 cells and yet I still get the same results.

Can anyone suggest what should I do to improve my model?

Sham.

Re: help
 

Without knowing anything about your model, the standard response is to check your grid scale and your reference values.

If those don't fix it, you need to describe your problem.

Goodluck, Jason

Re: help
 

Hello Jason,

Basicaly I am modelling a pipeline in a steady flow(0.38m/s) and drag, lift and inertia coefficients as the outputs. The Re is 1.4 x 10^5. I use the k-e RNG model at first.

The experimental results for Cd is around 1.1-1.2 but I only get around 0.54. same goes for Cl.

If it is really a problem with reference value(which I do not think so), which values should I change.

Thanks for your advice in advance Jason.

Sham.

Re: help
 

Did you set your reference values to begin with? At a minimum you should have set your Velocity, Density, Pressure, Area, and Length...

Do you know what they used for reference values to get Cd of 1.1 to 1.2? If so, calculate the force you would get for Cd of 1.1 at 0.38m/s, then compare it to the results when you do Report->Forces... If the forces match but the coefficients are off, then it's a problem with your reference values.

If the forces don't match, then double check your grid scal... go to Grid->Scale... make sure the extents of your model listed in this window are the same as what you modeled.

If they still don't match, then you have to start breaking down the results... check your y+ values (internal flow, I'd say you want y+<1)... check pressure and velocity gradients... look for high gradients and see if you can refine the mesh to account. Maybe k-e RNG model isn't the best for this situation... I'm not sure, I rarely deal with internal flow, and when I do it's based on previous models.

Hope this helps, and goodluck, Jason

Re: help
 

Jason,

First of all thanks for the great explanation. I guess you are right. Let me tell you my problem specification;

I am modelling circular cylinder of 0.504 m in diameter with 0.38m/s current. The water depth is 40 m but I only model around 5m from sea bottom. Sea water density and viscosity is 1025kg/m3 and 0.00139 kg/m-s.

It is a 2d problem. As you said, I suppose to get force of 47N but I get 0.047N, which I guess just how you define the units. Its' alright. But this time, the Cd and Cl is even less even though I have put the specified ref values.

Pls lead me.

Sham.

Re: help
 

Jason,

I just found out that the offset of the Force is because of the reference depth. If I increase the depth to 100, I will get 47N. But waht does this mean?

Does reference values mean we are referring to something relative to our problem?

Sham.

Re: help
 

The reference depth is the distance into and out of the screen (it's the third dimension to calculate your forces)

The reference values are very important. In 2D, Fluent still reports forces and mass flow rates in complete values (N instead of N/m, and kg/s instead of kg/s-m)... when it integrates the mass flow rate or forces in the 2D domain, it multiplies it by the depth you define to get a total force/mass flow.

I believe the reference pressure is also used to calculate pressure differences across a surface when the pressure on the other side of the surface is unknown. If the entire pipe is exposed to flow, then this pressure would cancel out, but if you're only modeling half of the cylinder (the half of the cylinder protruding above the sea floor), then to calculate the lift force it uses this reference pressure as acting on the underside of the surface.

All of the other reference values are used when calculating your coefficients.

Cl = Lift/(1/2*RHOref*Vref^2*Aref), etc... Any Fluid Mechanics text book should have the coefficient equations you'll be working with.

Hope this helps, and goodluck, Jason