Hi I am trying to simulate 2-d unsteady flow over a NACA0015 airfil.The simulation should be able to show the vortex shredding too.It's an incompressible flow (M=0.18),15 angle of attack,Hi Re number,I am using my finest grid, C-type,with a value of (y+)=1.Op. Conditions, Pressure=0.I tried several turbolent model but i think LES or DES is the best.inlet BL is inlet velocity and outlet BL is outflow.Do you think I've chosed the right model and the boundary conditions and etc.?Am I doing something wrong? is there any suggestions about this simulate? any suggestions would be very very welcome. thanks

I haven't seen outflow used successfully for external aerodynamics... only for internal flow where the BC is WAY downstream of any geometry changes. I would recommend switching to a pressure inlet/pressure outlet combination. If you turn on the energy equation you can use a pressure-far-field condition for your inlet and outlet (assuming you are far enough away... probably 10 chords fwd, above, and below, and at least 20 chords downstream since you're dealing with separated flow). Also, if I'm not mistaken, you don't have any pressure inputs in the velocity inlet or outflow BCs, and if you set your operating pressure to 0, then your defining your static pressure as 0, whereas if you use a pressure inlet you're defining a pressure in the BC so you can get away with leaving the operating pressure at 0.

M=0.18, I would recommend the segregated solver, especially with separated flow. You should be able to leave the URFs alone, as long as you set a pretty tight range on the limits for pressure and temperature (I usually use Pmax = Pstatic + 2*Q and Pmin = Pstatic - 3*Q... then I can estimate a temperature range that goes along with this pressure range).

I'm not very good at picking turbulence models. I usually have to ask people that are more experienced than myself. I would think LES or DES is a good assumption, but those require very refined meshes. I think you can coarsen the mesh some over the requirements of LES and use the Reynolds Stress Model (it won't be a huge mesh coarsening, but might be enough to make a difference).

Hope this helps, and good luck, Jason

Hi Jason, same circular cylinder case..Re=1e5, velocity=72m/sec,Dia of cylinder=.01m..this satisfies the Reynolds no. Requirement is unsteady DES simulation through Fluent...Grid is fine..I have Velocity inlet, pressure outlet, both sides of cylinder as symmetry and top and bottom as pressure-far-field. (Note that I have to assume ideal gas because of pressure-far-field) Now, I have tried through segregated/coupled solver with time steps of 0.035 timestep and 20 iteration for each time step..But it diverges from the very beginning with NAN (division by 0 etc)... What should be the approach.....?(decrease time step..run intially with RANS or steadycase and acheive certain amount of convergence in the domain) Cheers Endee

Different things could be causing the error. Double check your operating pressure and the pressure and temperatures you have in your pressure-far-field condition. If both pressures or the temperature are 0, then you'll have that error (P = rho*R*T, so P or T can't be 0 or rho is either 0 or infinity). Also, you say you have Velocity inlet, then you say you have Pressure Far Field. You have to be careful when combining BCs. I don't recommend letting a pressure-far-field BC touch any other BC except symmetry or periodic due to a non-continuity where the BCs meet. If you're using a Velocity inlet, then your pressure outlet is correct, but if you're using Pressure-Far-Field, I would recommend switching the outlet to Pressure-Far-Field as well.

I don't think you want to use a symmetry BC for this model. If I remember correctly, you're looking for unsteady effects like vortex shedding, correct? The symmetry condition will not allow you to predict vortices. A symmetry BC is basically a mirror... the vortices you're trying to shed will simply run into it's own reflection. You should model the entire domain if you're trying to get unsteady effects. If you're not trying to get unsteady effects, why are you using an unsteady solver?

IMHO: For 72m/s at standard atmospheric conditions, you're only talking Mach 0.2ish, so you should be using the segregated solver. The coupled solver is a density based solver, and since you're in the incompressible region, density variations are negligible and this will cause problems when solving with the coupled solver. Also, the variation in pressure between freestream and the separated flow behind the solver is difficult for the coupled solver to work out. The segregated solver is a pressure based solver, so it's ideal for incompressible regime flows, and especially flows with large separation regions.

Hope this helps, Jason

I have chosen segregated solver with PISO P-V coupling, Operating pressure 101325 Pa, Operating Temp 300K. Symmetry I had chosen just to cater for the length of cylinder as it was to be 1-4 dia to length but I have reduced it to 1-2 with symmetry on both sides. I have now removed the symmetry condition. If I implement the wall condition here..the wall effects will worsen the situation..due to reduced length, wall effect will be more pronounced? 2) Do you recommend to switch to Pressure Inlet BC instead of Velocity Inlet? If yes... what should be the corresponding Inlet Pressure at temp of 300k (As due to specification of Pressure-far-field i have to keep the ideal gas asssumption (which is ok as the flow is incompressible). 2. I am keeping the time step size as .035 with 20 subiterations (I am not yet able to see, due to divergence, that whether 20 sub iterations are enough for reasonable convergence or not). Is not this time step too big? 3. What should be the data saving interval to see the shedding of vortices? As the data size is quite big and i have to be selective with data saving frequency.

Thank a lot for your very kind guidance. I am highly obliged. Endee

Ok... I screwed up. I thought you were running a 2D simulation. Reading your last post over again, I understand what was going on with the symmetry condition. I apologize, but your symmetry condition will work here.

I think .035 seconds is big for your model. Assuming the center point of the vortex traveled at the same speed as the free stream, it would've moved 2.52 meters in .035 seconds. Seems to me that would be too much for one timestep, but I'm not too familiar with unsteady calculations, and I'm not sure what the time step should be.

For the right time step and model setup, 20 iterations should be plenty.

Ok... as far as Boundary Conditions... I would recommend either switching the Velocity Inlet and Pressure Outlet to Pressure-Far-Fields with the same conditions as the Pressure-Far-Field that you are currently using (but you have to make sure your outlet is WAY downstream of the cylinder... at least 20 diameters), or switch the current Pressure-Far-Field to Pressure Outlet and the Velocity Inlet to Pressure Inlet (from the Fluent manual, velocity inlets are "intended for incompressible flows, and its use in compressible flows will lead to a nonphysical result because it allows stagnation conditions to float to any level"). The velocity inlet with the ideal gas law could be part of the problem. You might be able to keep the velocity inlet if you switch the pressure far field to pressure outlet and turn off the ideal gas law. As far as calculating the inlet pressure, it's simply the total pressure (P0 = Pstatic + 1/2*rho*V^2).

Hope this helps, and good luck, Jason

Sorry to interrupt. I am doing unsteady application in 2D in a NACA 0012 at alfa=0 trying to get the same results as the NACA Report from Dr Abbot. Mainly my problem is to get the same drag result.

About that I've been using many meshes with diferent refinement, but the drag value is the same with S-A turbulence model.

The Reynold number is 1e6 using a 1 meter chord lenght wich gives a 14.607347 m/s in the velocity inlet BC. Operating pressure of 101325 Pa in a corner of a mesh to avoid static pressure that arfoil produce.

The value of Cd=0.00536 adimensional and CdForce=.5*1.225*14.607347^2*.00536= 0.7 Newton and I Fluent gives 2.56 Newton, far away what I do have to get.

Also I have tryied to use the RSM and the Drag value rise up to 5 Newton, the behavior of this is weird.

Do you have experience about? Thanks in advance Sebastian

Did you set up your reference values (Report->Reference Values)?

Jason

Many thanks, now I am winning playing a bit with the Turbulence Viscosity Ratio from 1 to 10 the value recomended for this. Anyway, thanks indeed.