transient simulation of supersonic nozzle
 

Hello,
I am trying to simulate a 2D transient flow in supersonic nozzle (with present shock wave). The inlet pressure is 10bar (1 000 000 Pa) and the outlet pressure is only 1 Pa. I am using density based solver and inviscid model. Geometry and mesh is in the attachement.

It seems that Fluent (version 2020R1) is having problem initializing the solution. Since I need to see how the flow develops in time I believe it is necessary to set initial values from the outlet (1 Pa everywhere in the flow domain). For the same reason it is also not possible to initialize the simulation with values from steady simulation or use a hybrid initialization.
To get a solution that does not totally diverge I need to choose a time step much smaller than the one that corresponds to recommended value according to fluent manual (delta t = typ. cell size/ velocity – this is in my case about 1e-9 s). Even by choosing time step 1e-13 s I do not get a converged solution.

I already tried using adaptive time step, mass flow rate inlet/outlet and dynamic mesh but nothing helped.

Does anyone have an idea how to fix this?

It's not a problem with initialization... you just have general convergence problems.

I probably wasn't entirely clear, sorry for that. What I was trying to say is, that if I use different initialization (for example I initialize the solution with values from steady simulation or use values from inlet - pressure 10bar) there is no problem with convergence.

Anyway, I could still use some tips, since I don't have many experience with transient simulations.

your mesh quality seems to be not good enough, look for boundary layer / prismatic layer
there is a bunch of threads on forum regarding simulation of exhaust from nozzle, you may check them

Hello Alexandr

thank you for your answer. I though that if I run simulation with inviscid model it's not necessary to use boundary layers. This simulation should be like the first step and once it is converge,d I am going to run another simulation with turbulent model using different mesh to get physically more accurate results.

Agree, prismatic layers are useless with inviscid model. Also the mesh quality is definitely okay.

So your inlet pressure is 10 bar and outlet pressure is 1 Pa or the inlet is 10 bar +1 bar and the outlet is at ~1 bar?

Seems anyways tricky to converge a transient run. Consider that in the initial moments your inlet is at 10 bar and the next cell is at 1 Pa, so you will have a massive pressure gradient producing equally massive velocities. So basically I don’t know where you got your velocity value to estimate the courant number but it is definitely wrong.

This pressure jump front should then travel from inlet to outlet and establish a reasonable pressure field. Your transient simulations must correctly resolve that, and you also need a very fine mesh following the pressure jump when it travels through the nozzle.

What you call “first step” to me looks very non trivial and requires a lot of work. So no surprise that you pushed the button and the CFD didn’t work. To be fair, the “second step” which is turning on the turbulence model, seems much easier

If i had to take a guess, The first ingredients you need is some very very VERY VERY VERY low time step to capture the velocity increase I mentioned you. This time step can probably increase with a ramp. Then perhaps, some dynamic mesh refinement to follow the pressure front

Dear LoGaL, thank you very much for your advice, I will try that.

Just for clarification:
1) yes, the pressure is set the way you said
2) concerning the choice of timestep, I assumed the lenght of the cell side to be of order 1e-4 m and the maximal velocity not to be more than 1e5 m/s. Is there something I am missing or is my guess just wrong?

So when you run it with 1e-14 (just first time steps eh!)what does it happen? Which settings are you using for the transient run? Simple, piso, coupled? How many iterations per timestep?

Hello again,

I tried what you suggested and unfortunately it didn't solve my problem completely... The good thing is that I don't get the error because of "excessive temperature change".

With this tiny time-step the first part looks fine but if I try to put slightly larger time-step residuals stop oscilating (see the pictures in attachement please I also made a screenshot of my settings).

Also a weird thing is that even if I let the simulation run for quite a long time (about 5000 timesteps) the contours of pressure stays the same but others change a little bit...

So, if I understand the plot, your residuals are now dropping by several orders of magnitude each timestep, which is good. You are now concerned that basically nothing changed, but this is not surprising, beause the timestep is very low and you ran only maybe 100 timesteps

You would theorically like to increase your timestep, but 2-3 things stop you.
First one is accuracy, but you can judge it with some CFL number plot and try to keep yourself around 1 in the zones you are interested into.
Second one is convergence at each timestep: your residuals must drop, say, 4 orders of magnitude. If the timestep is too large you might have noticed this does not happen.
Third one is that your solution might blow up.

2-3 have to to with the time step size and the settings you are using (e.g. Coupled formulations allow you to use more aggressive timesteps, SIMPLE and PISO are most preferred for high accuracy usually)


As I told you, it's not trivial to converge your simulation so you should not expect to push some buttons and hope it works. Once you headbutt that enough, it will work because you certainly have all the skills to make it work. Then turning on turbulence is very easy.

Make more tries, I am not sure you understand exactly what you are doing (For example, why first order time integration??? ). I don't think there's a cooking recipe that you can apply without thinking

So, to answer your questions...

Yes, my residuals are dropping but they eventually stop and stays at the same value which is not satisfactory (second picture of residuals at the last post), also I tried not to raise the time step and the result was the same...

Yes, I need to increase my time step because this way it would be almost impossible to run the whole simulation (even with cluster).

I am aware that the problem I am trying to solve is not easy at all, but I tried numerous ways to reach the convergence and failed in all of them. Also I am new to transient simulations, I tried to collect as many information as possible from Fluent guide, but I lack the experience, so it is definitely possible that I am missing some important detail.

So I would like to ask, where can I set the coupled formulation, I was looking for it in fluent and wasn't able to find it. Is it possible that it s not available for density based solver (which is the one I used)?

And finally, I chose first order time integration because I thought it is better to use higher terms only after I get converged solution with first order, because first order is usually more stable.

Thanks for your advice, i really appreciate it.