Compressible flow simulation at mach .7
 

This has probably been asked before, but a search didn't seem to help me all that much.

I have a model that I'm attempting to run in compressible mode, but it's diverging horribly.

My initial conditions are based off of a incompressible run which is converged to under 1x10^-4 continuity with the second-order solver.

This solution was run with these conditions:

operating pressure: 218 hPa
air density: 0.3507 Kg/m^3
velocity inlet @ 225 m/s on front face
outflow on rear face
symmetry for surrounding faces
wall boundary for the body of the object

For the compressible runs, I set all of the domain boundaries to pressure-far-field with:
gauge pressure: 0
temp: 216 K
mach #: 0.7
momentum along +x vector

I then patch the domain, setting domain temp to 216K

I'm running the simulation pressure based, cell based, and inviscid

I've tried density based as well and it does the same thing.

It begins warning that it's limiting pressure in certain nodes to 1, then it detects divergence and starts dropping the Courant number and timestep for some cells. Finally the temperature in some cells starts to spike and has to be limited. The whole time residuals are spiking. If I let it continue, it finally dies with a NaN error in the thermal solution.

Any ideas of what could be the culprit or what to change/modify to make it happy?

there might be several reasons for the problem.
firstly you probably have to use density based/implicit solver.
second, the outer boundary should be set to pressure far field
check the operating conditions and set the operating pressure to ambient pressure.
you do not need to patch the temperature for the domain.
the mesh for the case should be somehow a fine mesh.
the total pressure is the sum of static and DYNAMIC pressure. so consider it!:)

All of my outer boundaries are set to pressure far field and a gauge pressure of 0 hPa. I've also set the thermal component to the ambient air temp (216 K) and the momentum vector to point in the +x direction.

The operating conditions have the ambient pressure set to the proper value.

I did attempt another run using K-omega turbulence for viscosity and the density based solver and it was MUCH more stable. There was a rather large initial spike in residuals, especially the energy, but it ran steadily for 1000 iterations last night.

Now the problem is that it ran for 15 hours and residuals dropped less then an order of magnitude.

Any thoughts on how to get it to converge faster, or should I just let is churn all weekend?

that is sth. related to the mesh size and also the system RAM and CPU.
if your system has a kind of multi-core CPU, you can use the parallel computing ability of the software and get smaller times per iteration.
also, generally you can change the courant No. (control/solution panel) and set it to greater values. of course that depends to the case and greater than 5 values for the number may cause the case to diverge!

Right now I'm running the solution on 4 cores (of a 16 core cluster) with 62 gig of ram. I don't have enough licenses to use more cores. The mesh I'm working with is 6.5 million elements.

Besides courant number, is there anything else I can tweak? Any of the under relaxation factors?

edit: I may have found something. I used a incompressible solution converged with a second order flow solver and I didn't change it back to first order before I started iterating. I switched it over to 1st order flow and it seems to be converging fast. I'll have to let it run a few hours to be sure though.

hi,

I am sorry if i have missed something but from the discussion above it is slightly unclear what is your geometry . You said you intilisalised the compressible run with the inputs of the incompressible flow ( which is ok )
here is something i really did not get it

"My initial conditions are based off of a incompressible run which is converged to under 1x10^-4 continuity with the second-order solver.

This solution was run with these conditions:

operating pressure: 218 hPa
air density: 0.3507 Kg/m^3
velocity inlet @ 225 m/s on front face ??? ( did u input this for incompresible case set up ??, if yes then why
outflow on rear face
symmetry for surrounding faces
wall boundary for the body of the object "

What turbulence model did u use ??


Thanks for your reply

ciao
pratik

When I switched to compressible, I changed all of my boundaries to pressure-far-field. I input the ambient air temp, kept the gauge pressure at 0, set the mach number to 0.7 and made sure the momentum vector pointed in the +x direction. So the initial solution for the compressible run consisted of the incompressible solution for the inner cells of the domain and new boundary conditions.

I am using the K-omega turbulence model with the default values.