[Supriya_GM]

Hi,

I'm using FloEFD to recreate a convergent nozzle analysis carried out in a published literature that uses ANSYS fluent.




https://drive.google.com/file/d/0B4Y...ew?usp=sharing

The model in the image is what I'm trying to recreate in FloEFD. I carried out the analysis in two methods.

Method 1
I created lids at internal flow inlet BC and Outflow BC.
The boundary conditions are specified at 101325 Pa static pressure at outflow BC and 162120 Pa (= 1.6*101325) total pressure at inlet BC. 101502 Pa total pressure at ambient inflow BC and 101325 pa environmental pressure at far-field BC. ( the published literature also considers M= 0.05 at the far-field boundary which I wasn't able to specify). The total temperature remains 288 K at all regions. These boundary conditions are as given in the published literature.

The results obtained using this do not match the Fluent analysis. I compared Cd (Flow Coefficient), Cfg (Gross thrust Coefficient) and Total Pressure Recovery Coefficient.

Method 2
I modelled only the nozzle without the domain. Created lids at inlet and outlet of the nozzle. The boundary conditions were specified as 162120 pa total pressure at inlet and 101325 pa static pressure at outlet.

Analysis using the method 2 yielded results that closely matched the Cd, Cfg and total pressure recovery coefficient of the published literature.

Here are my questions,

1. Is the method 1 correct? I'm sure I'm not assigning the boundary conditions correctly. What is the right way to assign boundary conditions to this model?

2. Is the method 2 correct?
Some reading on the theory of convergent nozzle made me understand that if the flow reaches sonic values, the total pressure at the exit plane is equal to the critical pressure which is 0.5282 times the total pressure at inlet. In the analysis flow at the exit reaches sonic value.

I am able to achieve this value at the exit plane using method 2.

Also, FloEFD says for outlet pressure boundary conditions, if the flow reaches sonic values the outlet pressure has no effect. I believe this is the reason why method 2 is anyway yielding close results.

3. Theoretically does assigning 101325 static pressure at the nozzle exit or further downstream in the domain make a difference ?

Thank you

[Boris_M]

Hi Supriya,

1.
This case, in general, I would not have considered as an internal case. Although it is described in FloEFD workings almost as an internal case with the boundary conditions, it is more of a typical traditional CFD case description.
So I would have chosen Method 2 as it is an external case.

2.
Yes, an external consideration is correct. The 1.6* 101325Pa corresponds to the dynamic pressure portion in the total pressure of the 0.05 Mach number flow. In an external flow, there should be no problem to have any supersonic outlet flow condition. You should just avoid any outlet lid/opening, a free stream out of the computational domain such as in an external flow is not an issue.

3.
This probably relates to the internal case as in an external case I would not specify an outlet lid with a pressure opening. At least not in the external space, if there is an internal duct in a simulation that also considers the external space for convection purposes for example, then the internal duct can have such a boundary condition but in your case, it is a purely external task.

The M=0.05 can be specified in the external case in the initial conditions of the general settings so the flow itself has the properties and the far field boundary conditions are just static pressure plus the M=0.05 from the flow field. But in your case the nozzle geometry looks odd shaped on the outside for the flow to cause disturbances if you would consider the nozzle as part of the external flow. This is why a solid block should be modelled with the nozzle carved out of it. So basically everything left of the "Ambient Inflow BC" is solid except for the nozzle and then you apply the flow BC on the ambient inflow BC surfaces. This solid block will extend out of the computational domain vertically just like in my example and the flow will flow out on the right open side of the computational domain. Please don't judge me on the nozzle design

I hope this helps,
Boris

[Supriya_GM]

Hi Boris,

Thank you for clarifying my doubts.
I will remodel my geometry according to your suggestion and run the analysis.

The nozzle used is a serpentine nozzle, whose centerline follows Lee Curve equation. This is an S shaped curve. This particular nozzle uses two S shaped curves and is a double serpentine nozzle. These are used to suppress infrared radiation signatures (IRS) emitted by engine exhausts.

Thank you for your input.

Supriya