Hi Dev, Glad to hear you are making some progress. In regards to your points:

On 2 Jan 2017, at 08:24, devabratasahoo@campus.technion.ac.il wrote: Hi Users, I am solving my cavity flow case at a Re= 0.3x10^7 per mtr, M=0.15, and NumModes=4. I am not using the CFL tool, instead I am taking aconstant time step = 0.0001. The simulation is running fine now but the problems now remains as follows: 1) The residuals are not good at all. (pics attached below)

The residuals in this case are not actually residuals -- the wording we use here is rather confusing (i.e. "L 2 error") so let me clarify what's going on. The idea behind this is that if you specify an exact solution in your session file, the solver will dump out the L^2 and L^inf norms of the error, i.e. you'll see the result of || u - u_exact ||. Clearly most of the time this is not available, so if you don't specify it then we assume that u_exact = 0. The figures you are seeing are therefore just the norms of each of the conserved variables.

2) I am still not able to capture the boundary layers in this mesh though the flow in cavity is captured but it can't be accurate. (Present mesh attached below)

This is (probably) due to the under resolution of the mesh at such a high Re. The boundary conditions in the compressible solver are only enforced weakly through the Riemann solver. We have found that in the presence of under resolved grids, there's too much diffusion of the solution field and therefore the boundary layer is unable to form. The only way you'll test this is to either drop Re or increase the resolution.

3) My final aim is to run the simulation at a larger RE (1X10^7 per mtr at M-0.5). (presently used solver info, parameters and expansions used are attached below)

Okay. Some suggestions: - as stated before you'll likely require additional resolution (and therefore a reduced dt) - you might also try to use a WeakDG advection type (this may be more efficient than the FRDG) - I highly suggest a more advanced Riemann solver, perhaps HLLC. The Roe solver is possibly adding to your diffusion issues at the boundary. There are a bunch you can try, see the RiemannSolver directory of the compressible flow solver source or consult the user guide.

4) I also need to run the CFL tool to get the mean flow which I can further use as base flow for the stability analysis. I am trying it out but the solution is terminating when I use CFL tool. It is working only when I use CFL=0.1.

The CFL estimator is probably not as accurate as it should be. I'm a bit confused as to why you need to use this however to obtain a mean flow? Cheers, Dave

1) Residual <residuals.jpg>

2)Present Mesh <Medium_Mesh.jpg>

3) Solverinfo and Parameters used <SolverInfo_parameters.jpg>

4) Expansions used

<Expansions.jpg>

Result(Mach Contour at 1Sec) <mach contour.jpg>

I tried the same case at a very low Re = 7500 using Incompressible flow solver and I could capture the boundary layer but the residuals still not good. When I try running it for longer time the solution is blowing up. Can anyone please help me out with where I am going wrong? How to reduce the residual and get a converged solution?

Regards, Dev

_______________________________________________ Nektar-users mailing list Nektar-users@imperial.ac.uk https://mailman.ic.ac.uk/mailman/listinfo/nektar-users

-- David Moxey (Research and Teaching Fellow) d.moxey@imperial.ac.uk | www.imperial.ac.uk/people/d.moxey Room 364, Department of Aeronautics, Imperial College London, London, SW7 2AZ, UK.