waves of values in supersonic flow
 

Greetings,


I get very strange results from a supersonic compressible CFX-simulation.
The geometry you can see in the attached picture. The Inlet and outlet are the periodic faces.


There is a shaft with two walls and two symmetry boundaries. The inlet and outlet are connected with an interface. The velocity is generated a subdomain with a momentum source (Domain->Subdomain->Source->Momentunm Source->x Component = 100000 kg/(m²s²)) It is enough impulse to accelerate the flow up to 1,4 Mach.
But from some reason waves in values get produced, see picture 1. They can be observed in the density, temperature and pressure field. When I turn off the compressibility they do not appear, so it has to do with that.

Turbulence model: SST
Advection Scheme: High Resolution
Turbulence Numerics: First order
Wall Heat Transfer: Adiabatic



Of course the calculation gets an overflow and crashes. After quite a lot iterations, but the waves can be observed already after view iterations.



Does anybody have a clue why I get such results and how I fix my setup?

Attachment 58378


Thanks

density based
 

Is the maybe I shall somehow change the solver to density based. Is it possible in CFX? Is CFX otherwise pressure based?

CFX does not have a density based solver. Only Fluent has that.

Are you aware that compressible frictional flow in a duct results in more than just pressure drop along the flow direction - the temperature and density changes as well. https://en.wikipedia.org/wiki/Compressible_duct_flow

As you have not specified any source term to control the thermal field I am not sure whether this flow is actually periodic.

Thank you ghorrocks for the fast response.
Of course I'm aware of the basics of fluid mechanics.
Please note, that the change in the values happen not along the flow direction, but perpendicular to it. The Inlet and outlet are the periodic faces.

A heat source is not planned. I just initialized the calculation with a temperature of 500K. Because the walls are adiabatic no energy gets lost.
The momentum source compensates the pressure lost through friction at the walls.

I already ran this simulation with a smaller source and a low velocity (<0,3Ma) and there were no problems.

They say, that supersonic flows should be simulated with a density based solver. But where is an analogical setting in CFX?

There is no analogous solver to Fluent's density based solver. CFX has one solver for all flows.

The reason I pointed to the compressible flow link is because it shows the temperature changes in the flow direction as well. This means the flow is not periodic. So you are modelling the flow using a setup which cannot handle the actual flow, so weird things can happen. So I would not bother about fixing waves in a model which is non-physical in the first place. The non-physical simulation is a more fundamental problem.

A very interesting explenation.
The peridicity is used here in order to observe a fully developed boundary layer without modelling the whole inlet length of the duct. So it shows just a small section of an imaginary pipe.

The case and the approach are given from the professor. I'm not allowed to change it. But I have to solve it.

Sent from my SM-A510F using CFD Online Forum mobile app

Yes, using periodic boundaries is a standard way of modelling fully developed flow. But compressible flow in a duct is never fully developed (well, not until it gets Mach 1 and then stays there). And that is your fundamental problem. You can't use a method for fully developed flow to model something which is not fully developed.

You can tell your professor that his problem is not solvable :)