[gerogero7]

Hi everyone,
I need some help with a simulation of a combustion chamber with conv-div nozzle for space application. I have a simulation with a non premixed combustion with two mass flow inlets and with a pressure outlet (with the exit gauge pressure I got from gasdynamics). The operating pressure I set is 0 Pa cause it's designed to work in space (I am not anyway sure if this last statement is correct).
The main problem is that even though the simulation converges pretty well, I have a backflow in the 75% of the outlet which is inappropriate given the physical situation. The first part of the residuals was with everything at first order upwind then, after the spike I tried to chage everything to 2nd degree to see if anything changed.
The mesh is a 370k elements hybrid mesh (it is unstructured only in the section with a radial inlet). The strange thing is that a 25k elements unstructured mesh worked pretty fine even if I got a strange high boundary layer in the divergent (using k-epsilon std). Now I am using K-w-sst to better capture the b. layer.

What should I change to eliminate that backflow?

Thank you for your time
LG

[vinerm]

If the modeled length of the domain is its actual length, then the flow reversal is also exist in reality. It is not so that the flow reversal is always numerical; it exists in real scenarios. So, if the outlet of the nozzle is located where it should be, then flow reversal is part of the solution.

[gerogero7]

First of all thank you for your response.

Yes, the model should be of that size.
I am not catching the linking point between the paper and calculator gasdynamics and the results of this model, which is not representing the physical reality of a divergent nozzle expansion in the void of space.
Could you give me some clue? I am still sure that the problem is in the setup of my CFD model.

Thank you again
LG

[gerogero7]

For comparison this is what I expect. Even though the boundary layer in this model is still too much thick.

[vinerm]

This also has flow reversal. What pressure value are you using at the outlet? And how are you modeling the gas density?

[gerogero7]

I am using a pressure of 315 Pa (as from the area rule, given the total pressure in the chamber which is 3.63 bar)
The gas density is set as "pdf". I suppose it is using a compressible flow with the properties of the gas coming from the local composition of the mixture.

[vinerm]

Pressure does not get divided by area; force gets divided to give pressure. So, you need to apply 3.63 bar and not 315 Pa.

[gerogero7]

So the setting for the outlet pressure is the total pressure of the flow or the local pressure it has as taken from gasdynamics?

Anyway i set the condition you suggested but it doesn't get better.
What do you think?

Further informations: as operating pressure i set 0 Pa, the gauge pressure for the two mass flow inlets is 0 Pa as well. The spike in residuals is for the change of order to quick

[vinerm]

You cannot use 0 Pa anywhere, either at the inlet or at the outlet. All pressure values should be positive. If the pressure in the chamber is 3.63 bar, then pressure at the inlet would most likely be higher, until unless it is a diffuser, which it is not. Similarly, pressure at the outlet will have some positive value and the density depends on that value.

[gerogero7]

Good morning, and thank you again vinerm for your help.
I have set up a simulation with the boundaries you suggested. Now there's no more the problem of the reversed flow. But i still get a pressure slightly higher than the gasdynamics one (3.9 bar vs 3.6) and the contour of mach in the nozzle has that radial evolution instead of the expected axial evolution.

Operating press is 0 Pa, pressure outlet is 315 Pa, in the non premixed combustion I set compressibility effects with equilibrium press ot 3.6 bar, the mass flow inlets have both a pressure of 4 bar. Am I missing something?
What do you think?


Kind regards,
LG

[vinerm]

That's most likely because you have 4 bar at the inlet. And is 315 Pa correct value for the outlet? It appears to be too low.

[gerogero7]

From the area rule i find an outlet mach of 4.64. With that and with the chamber total pressure (stagnation press) i find that the static pressure at the outlet is 315 Pa.
Clearly the total pressure at the outlet is still 3.63 bar as in the chamber.

What should I impose? With 315 Pa i have that strange pattern i showed you. With 3.36 bar i have backflow on 63% of the outlet.

Thank you for your help
LG

[vinerm]

I don't know what you mean by area rule, but if 315 Pa is based on isentropic relations, then it should be alright. But why do you have 4 bar at inlet? If total pressure is 3.6 bar, then it should be same at the inlet as well. Total pressure should remain constant. Since you are using mass flow inlet, the pressure at the inlet is supersonic pressure, which should be close to 3.6 bar, however, this value is used only if the flow is locally supersonic.

[gerogero7]

Sorry, I call it area rule, but actually those are the isoentropic relations.

Ok, to summarize what now I have:

- massflow inlet fuel: 3.6 bar & massflow value
- massflow inlet ox: 3.6 bar & massflow value
- pressure outlet: 315 Pa
- operating pressure: 0 Pa
- combustion: non premixed, w/ compressibility effects @ 3.6 bar operating press, flammability limit 0.17

and what i got from the last simulation with the aforementioned conditions:

- residuals have reached at least 1e-4 in each quantity (1000 iter)
- no backflow or min pdf enthalpy

but:

- a relevant volume of the combustion chamber has a pressure ot 2.7 bar
- the nozzle has the same issue as always as you can see from the image
- the total pressure changes a lot passing through the nozzle (strange) as you can see from the other image

Kind regards,
LG

[vinerm]

Total pressure remains constant in a system where you don't have energy addition or extraction. In reacting flows, there is energy source, hence, total pressure is not supposed to remain same.