[Shamoon Jamshed]

Dear CFD enthusiasts,

I am simulating a case of the jet flow confined between two walls (see figure please). a jet is tilted towards the right wall. i am not understanding that the temperature is quite restricted at the lower region of the right-wall while the left wall is fully showing thermal gradient. Is this phenomenon normal? Currently, I have given pressure inlet for jet and velocity inlet for the confined gap between two walls ( very low velocity was given). The solver is pseudo transient with pressure based coupled setting and first order for all the equations. PS time step is 0.1.

Please help.

Regards,

SJ

[Shamoon Jamshed]

any one to help? please, its a bit urgent

[AlexanderZ]

what results did you expect?
what is the temperature of gas flows out of the nozzle?

[LoGaL]

The simulation doesn’t seem converged

[Shamoon Jamshed]

@AlexanderZ, I was expecting the opposite behavior of the walls, since the right wall is more closest to the flame, it should be warm till its top. while the left wall should be much cooler. Temperature at exit of the nozzle is around 1500 K

[Shamoon Jamshed]

Originally Posted by LoGaL

The simulation doesn’t seem converged

at first i also thought, but the residuals converged til 1e-04. while others (Turb, momenutm, energy) conveerged more than 1e-06.

[Shamoon Jamshed]

please anymore help is appreciated.

[LoGaL]

continuity to 1e-04 is not converged in my opinion. And that weird vortex you have in the simulation makes me believe it even more so.

[LoGaL]

to make myself clearer, i attached a picture. Usually you get weirdos like this when the simulation is not converged. Could you please place some points inside the domain (especially in the zones i am pointing) and monitor velocity and temperature there for some iterations (say 500-1000)? I expect them to oscillate.

[Shamoon Jamshed]

Originally Posted by LoGaL

to make myself clearer, i attached a picture. Usually you get weirdos like this when the simulation is not converged. Could you please place some points inside the domain (especially in the zones i am pointing) and monitor velocity and temperature there for some iterations (say 500-1000)? I expect them to oscillate.

so what are your suggestions

[Shamoon Jamshed]

Originally Posted by LoGaL

to make myself clearer, i attached a picture. Usually you get weirdos like this when the simulation is not converged. Could you please place some points inside the domain (especially in the zones i am pointing) and monitor velocity and temperature there for some iterations (say 500-1000)? I expect them to oscillate.

I used pseudo transient, and using large pseudo time step makes the simulation diverge. After seeing the initial comments on CFD-online, when i switched to density based coupled after 10k iterations of pseudo time step (pressure based coupled), this vortex removed. but still satisfactory results are not obtained , since there is still a blue dominant region on the wall.

[LoGaL]

Pressure based pseudo transient with 0.1 multiplicator is fine.
My suggestion is that you first check if my guess is correct by monitoring the temperature and velocity at different points as I suggested, then if I am right, we decide what to do

And, just to be clear, it is really hard to give you suggestions, because you provide just a temperature contour as input. I can barely understand what is your setup.

[AlexanderZ]

show the cross section with velocity and temperature contours.
use the axis of nozzle as plan guide and make it perpendicular to walls
so we can check flow distribution in domain

[Shamoon Jamshed]

Originally Posted by LoGaL

Pressure based pseudo transient with 0.1 multiplicator is fine.
My suggestion is that you first check if my guess is correct by monitoring the temperature and velocity at different points as I suggested, then if I am right, we decide what to do

And, just to be clear, it is really hard to give you suggestions, because you provide just a temperature contour as input. I can barely understand what is your setup.

I am simulating a jet flow with 54.5 bar pressure of air. The jet is confined between two walls. the walls are adiabatic. the walls are along three sides but the fourth side is pressure outlet. The domain other than jet are given velocity inlet . ( and you are welcome to suggest here the BC because actually, there is static air here while the flow is coming out of the grey geometry as shown in figure). I gave the velocity inlet of 1m/s just to run the flow in the domain other than the jet.

[LoGaL]

Ok I see. You should specify a pressure inlet instead of velocity, if you know the pressure inside the chamber. I would actually recommend it, because by imposing velocity inlet you are kind of forcing the mass flow, which is unphysical

Anyways, I have some experience with nozzle flows and, as I said, I expect the steady simulation to not converge very well. Is it also supersonic? The pressure jump is quite large.

So please, place those points inside the domain and monitor temperature and velocity for ~1000 iterations, so that we see if the solution oscillates. If it does, usually one makes sure to have a good quality mesh (show me skewness and orthogonal quality) and if that is the case, the usual procedure is to run an unsteady simulation with low courant number

I’ve seen sometimes that turning off the curvature correction in the turbulence model can stabilize the solution but, in my experience, for so high pressure jumps you must run unsteady. Especially since you are running everything with first order (which I don’t recommend), I don’t expect that turning off curvature will do that much, as you are already trading accuracy for stability

[LoGaL]

I post you a pic of my thesis of 2 years ago to give you the idea of what I have in mind. The topic was about fuel jets with real gas effects into a chamber with air... pretty similar if you ask me

So you see that I was monitoring sound speed at a certain point in the domain. The steady solver oscillated a lot, (and the solution looked real weird) but when I turned on the transient solver, everything stabilized.

I guess you have something similar, but if you don’t place those points and monitor, I can’t confirm

[Shamoon Jamshed]

Originally Posted by LoGaL

Ok I see. You should specify a pressure inlet instead of velocity, if you know the pressure inside the chamber. I would actually recommend it, because by imposing velocity inlet you are kind of forcing the mass flow, which is unphysical.



Anyways, I have some experience with nozzle flows and, as I said, I expect the steady simulation to not converge very well. Is it also supersonic? The pressure jump is quite large.

So please, place those points inside the domain and monitor temperature and velocity for ~1000 iterations, so that we see if the solution oscillates. If it does, usually one makes sure to have a good quality mesh (show me skewness and orthogonal quality) and if that is the case, the usual procedure is to run an unsteady simulation with low courant number



I’ve seen sometimes that turning off the curvature correction in the turbulence model can stabilize the solution but, in my experience, for so high pressure jumps you must run unsteady. Especially since you are running everything with first order (which I don’t recommend), I don’t expect that turning off curvature will do that much, as you are already trading accuracy for stability

1." I specified the pressure inlet on jet and the side wise domains as velocity inlet which are in fact for static air outside of the jet.
2. For that, I must say that I ran the solution (initially) in two parts: first I ran the jet flow, then after convergence, I ran the static flow between walls with very low velocity. then i combined the two cases, by defining interfaces between jet and the static domains.
3.
4. i dont get very well this point, but I also tried an unsteady run which was nt very stable, so i had to return back to steady case.

[LoGaL]

1) What I am saying is that for static air in the chamber, you can specify pressure outlet everywhere instead of velocity. It is fine. Don't flush low velocity air inside the domain, just give it a pressure.

2) Please, Please, place those monitor points inside the domain and try to get a plot of the temperature and velocity like the one I posted you. Place them where the jet is expanding in the chamber. DO IT or we don't know if this is the problem. You will have to run the simulation a bit more.

3) Turn off the curvature correction option in the turbulence model and see if it improves the continuity convergence.

[Shamoon Jamshed]

Thanks LoGal for your help. And, by the way, how did i forget. I repeatedly get many turbulent viscosity ratio warnings too

[LoGaL]

this confirms me even more that your simulation is not converging.

Please, the monitoring of velocity and temperature at some points where the jet is expanding in the chamber, or I can't help you.

And while you are there, also a picture of the mesh and the mesh quality (did you mesh it with the ansys mesher?)