[Balakrshnan Ramakrishnan]

do you use simpleFoam?

did you try to do without turbulence models?

[lovecraft22]

I only tried simpleFoam with turbulence models.

[Balakrshnan Ramakrishnan]

First : Try using no turbulence model. It will be easier to debug.

Second :

I cant understand why your k value is 0 everywhere and epsilon value is 1.78 ?? Any particular reason behind this?

[lovecraft22]

Originally Posted by Balakrshnan Ramakrishnan

First : Try using no turbulence model. It will be easier to debug.

Second :

I cant understand why your k value is 0 everywhere and epsilon value is 1.78 ?? Any particular reason behind this?

Nope, no reason, just copied them over from the motorbike tutorial. Anyway setting the boundary as srakshit I now got some reasonable results!

Thank you to both of you!

[Balakrshnan Ramakrishnan]

Just for your reference in the future simulations please look into

http://www.cfd-online.com/Wiki/Turbu...ary_conditions

to set initial conditions for k , epsilon and omega..

Have fun

[lovecraft22]

Thank you!

[srakshit]

You have to define one pressure value at least.

I set the pressure value to 0 at the inlet and the rest as you suggested.
Now it's running, let's see what comes out.

Out of pressure and velocity you can define one. If you have defined velocity at inlet and outlet as 30 m/s, then i wont prefer setting pressure = 0.

This is because of 2 reasons
1. If at the outlet U is fixed at 30 m/s, pressure will be depend on what fluid you are using. At steady state, both inlet and outlet pressure should be in the same range (not much difference) because its constant velocity simulation.
2. If U and p are inconsistent then you will get inconsistent solution. More iterations you will run, higher the velocity inside the domain you will get. This is because flow will bounce between two Dirichlet boundaries with inconsistent pressure.

If you are thinking of setting pressure in either of the boundary, then you have to keep the velocity floating at that boundary (or you should define some physical value).

Results with flow over a cylinder with fixed velocity (U=30 m/s) and floating pressure can be seen in the attached images.

Yes, i agree with Ramakrishnan. Turbulent properties should be defined correctly and solving without them will help in identifying the problem.

[lovecraft22]

The same case won't converge with icoFoam… Why?

[srakshit]

Originally Posted by lovecraft22

The same case won't converge with icoFoam… Why?

It does, try decreasing the deltaT.

Also, check your ddtSchemes in fvSchemes.

[lovecraft22]

What should I check about the ddtSchemes?

[m2montazari]

hi,
as I had ran similar cases a lot, I think best condition is:
1- domain should be large enough and cell height at surface of cylinder should be small enough
2- boundary conditions should be as follows:
U: inlet: fixedValue, value=30,0,0
outlet: zeroGradient
cylinder: fixedValue,value=0,0,0
P: inlet: zeroGradient
outlet: fixedValue,value=0
cylinder: zeroGradient
k and omega: inlet: fixedValue,value=...(depend on your turbulence - you can use turbulence intensity instead of fixedValue also)
outlet: zeroGradient
cylinder:fixedValue,value=0 (for k)
fixedValue,value=a large number depending surface roughness(for omega)

3- discretization schemes should be limitedlinear or upwind (linear scheme makes fake pressure waves)

and about the pressure: most of CFD codes use gauge pressure to reduce errors because abs.pressure is usually a large number and its gradient is small, so roundoff errors increase with abs. pressure as calculation pressure. for incompressible cases as in N.S. and continuity eqn. there is no P, but just gradient of P, so any value for outlet pressure gives same result but a shift in pressure values in domain.

and about icoFoam, it is a piso based solver and should be ran with small timesteps. as your case has unsteadiness (because of vortex shedding and separation unsteadiness) you cant reach a steady converged solution but you can have converged unsteady solution after a reasonable time advance.

I hope these helps,
Mohammad