[Viento]

Mode: Trancient
Domain setup: Air ideal gas, Total energy, Laminar, Reference pressure = 1 atm.
Inlet: supersonic, velocity = 450m/s, relative pressure = 0pa, temperature = 300K.
Outlet: supersonic.
Initial conditions in domain: velocity = 450m/s, temperature = 300K.
Achieved convergence: less than 1e-04.

Hello. I'm trying to get a conical shock wave shape around the central spike (as it happens in the ramget engine), like this:


But I get a straight front, which spreads farther and farther from the central spike. Opposite the supersonic flow.

This looks strange and improbably. So, what I'm doing wrong with the setup?

[AtoHM]

Try to understand what you are looking at. What does the Mach distribution near the wall tell you? What happens to flow within a nozzle?

[Gert-Jan]

@ Alex
- why oh why do you try to run the most difficult case from scratch? That is asking for problems.
- why not try simple and increase complexity with every restart:
1) steady state; inlet vel = 10 m/s
2) steady state; inlet vel =100 m/s
3) steady state; inlet vel =300 m/s
4) steady state; inlet vel =450 m/s
5) transient; inlet vel =450 m/s

Don't try to hit the roof in one go, and expect CFX so solve all your problems in one step. It is not a panacea. That's a silly approach.

[urosgrivc]

first problem -> temperature = 300K, what fixed like isothermal? total energy ideal gas might be considered
Are those walls near the body and is the cone in the tube?
or are you are simulating a cone in free flow
what about axisimetry also do you have a 2d flat or axisimetric

[Viento]

Originally Posted by urosgrivc

first problem -> temperature = 300K, what fixed like isothermal? total energy ideal gas might be considered

It`s just a constant temperature of atmosphere entering the inlet. It changes within the domain.

Originally Posted by urosgrivc

Are those walls near the body and is the cone in the tube?

Yes, this is the cone in the tube.

Originally Posted by urosgrivc

what about axisimetry also do you have a 2d flat or axisimetric

It is axisymmetric. Sector is about 20 deg.

Originally Posted by Gert-Jan

3) steady state; inlet vel =300 m/s
4) steady state; inlet vel =450 m/s

It normally worked with all types of subsonic flow on steady state, but jump to supersonic flow on steady state persistently loses convergence and gives an error.

Originally Posted by AtoHM

Try to understand what you are looking at. What does the Mach distribution near the wall tell you? What happens to flow within a nozzle?

Hmm, this made me think a lot. Initially, tube was short. I extended the tube between the cone and the air intake to track the transient phenomena that caused an error in the first attempts of modeling. It seems that the cause is not in the cone, but in the walls, that cause critical phenomena in the boundary layer. Maybe I managed to reproduce something like this phenomenon with slowering the flow in multiple shock waves?

[Gert-Jan]

What you see in your figure is how CFX tries to recover from an initial guess of 450 m/s everywhere. As a result the flow is chocked between your obstacle and the wall. Therefore no more gas can get through which leads to corrections in the flow upstream. The velocity will decrease and it is likely that your inlet is blocked for 100%.

So your figures show how CFD tries to recover from a completely unrealistic initial condition with 450 m/s everywhere. You won't get very far with that as a start. Therefore you need to start slowly and ramp it up with increasing velocity.

You mentioned that you could not get it to supersonic flow using this approach. You have to try harder. If this is not going to work, then the approach shown above won't work as well.