Learning Forum

[Vinay Kumar Vemulapati]

"Artificial walls on 18 faces (1.4% area) of pressure-outlet 6 to prevent fluid from flowing into the boundary" while performing 2D analysis of Non reacting flow (i.e. no combustion). Also oscillation of Residuals.

Net Mass flow rate is nearly 0.

Mesh: 95,000 cells with inflation near walls

Model: SST k-ω

Boundary condtions

Inlet: Pressure farfield - Mach 2.0

Outlet: Pressure Outlet - (-1000 Pa), prevent reverse flow, Average Pressure specification

Solver: enabled high speed numerics

Initialization: Standard initialization and fmg initialization

[Federico]

Hello Vinay, 

You get the written warning because you have set the condition to Prevent Reverse flow. As a result, Fluent is creating "artificial walls" on 1.4% of your outlet surface area to prevent any flow from entering back through the outlet. This can happen if your outlet pressure is lower than the outlet BC over the course of simulation.

Regarding your residualts, can you show some contour plots of Velocity or Mach number?

[Vinay Kumar Vemulapati]

1. Should outlet conditon need to be lower than -1000 Pa?
2. Is it required to change flux type from Roe-FDS to AUSM. Most researchers used AUSM.

[Vinay Kumar Vemulapati]

Mach Number:

Pressure:

[Federico]

Yes, I would encourage you to use AUSM, which provides good shock resolution.

I cannot speak of the inlet/outlet conditions here, as this will be problem dependent.

[Vinay Kumar Vemulapati]

Can you tell about negative pressure near walls?

[Federico]

The static pressure in Fluent is a Gauge pressure, so it is relative to the Operating pressure that you have set. The default value for Operating pressure is 1atm, so the absolute pressure along the wall would be Static pressure + 1atm. Or you can plot Absolute pressure directly.

These pressure plots tell me that the mach number is higher in your simulation than the experiment. Why are you using -1000Pa at the outlet?

[Vinay Kumar Vemulapati]

Same outlet condition is used in ansys fluent ABP "Application Best Practices High-Speed Combustion Modeling with DLR SCRAMjet for For Ansys Fluent 2022R1".

 

[Federico]

Are those conditions the same in the experiment that you are comparing this with?

[Vinay Kumar Vemulapati]

Yes, but in numerical analysis they mentioned "Neumann boundary condition is used to define the outflow wall of the domain".

 Boundary Conditions

Variable	Air	H2
Ma	2.0	1.0
U (m/s)	730	1200
T (K)	340	250
P (Pa)	100,000	100,000
⍴ (kg/m3)	1.002	0.097
Y(O2)	0.232	0
Y(N2)	0.736	0
Y(H2O)	0.032	0
Y(H2)	0	1

 

[Federico]

What are you showing me with this table?

[Vinay Kumar Vemulapati]

Inlet conditions of experiment.

[Federico]

Are you using the same for your simulation? What is your gauge pressure/Temperature at the inlet? What are your operating conditions?

[Vinay Kumar Vemulapati]

Yes,

Guage Pressure = 0 Pa

Temperature at inlet = 340 K

Operating condition, Operating pressure=101325 Pa