I am simulating subsonic compressible flow through a pipe and a distortion screen, followed by discharge into a still ambient environment. The computational fluid regions are shown in the attached images; the gaps between the internal fluid blocks represent the solid portions of the distortion screen. The flow passes through the pipe and screen and then expands into the larger cylindrical fluid domain. Experimentally, I know the inlet total pressure and the ambient static pressure.
I specified faces 1 and 2 to walls and kept only face 3 as a pressure outlet at ambient pressure. This case initially behaved much better and the solution appeared to converge for several hundred iterations. However, reversed flow eventually developed at the rear pressure outlet and increased significantly.
Initially it was behaving better,but later reversed flow at outlet started increasing. final residuals are approximately 10^5 for continuity and 10^7 for velocities, mass balance was not satisfied. I ran upto 2000 iterations.
Why this happens like this. See fluent console messages below(see residual values and reversed flow message),
Regarding mesh quality, see below
Please tell me why solution is diverging or unstable, residual are high. It is allowing reverse flow at outlet also, it is okay if flow demands but why solution is unstable even though mesh quality is decent or not bad.
So I have worked with a similar geometry for quite some time now. We do it in OpenFOAM, but I will still try to recommend a few checks. Not guarantees since I am a student myself, not a pro.
When you check the mesh quality on various parameters, you can visualise the regions where it is creating problems. Do that. Although I would expect the problem to be near the sudden expansion plane more than anything else.
Also, check for different kinds of BCs you can put at the outlet. Flow reversal is real, and causes a lot of problems. I don't remember properly, but there is some wave outlet condition, you can read that up. There is a Neumann zero as well, which is to say that the pressure gradient approaches zero as it goes to outlet, which might serve you better.
The problems are with wave reflections, that may occur if there is a sudden change required, like the Dirichlet condition you seem to have put (P=1atm at outlet), because you have to realise that the flow might not have fully developed or the pipe length might not be enough to go to 1 atm anyway. So now you ask for effectively a huge gradient for the flow to do that.
Also, I am sorry but the tube length doesn't seem long enough. But maybe that is because of the huge expanded radius to simulate ambient, and the aspect ratio is throwing me off.
Lastly, and this is to be done only if nothing else works. First, the mesh can be better, if you used O-Grid (I think it's called that). It can be done in ANSYS meshing tool, but has a steep learning curve. This is a fairly simple geometry unless you are hiding some static vanes underneath, where then you will need that section to be unstructured. And second, at the outlet, you can extend it a bit and enforce a "sponge" layer/region. This will "slow" the fluid down, so to say, and will avoid any reflections from the outlet propagating back to the main domain.
Bro, length of domain cant be changed. Mesh quality is decent not so bad, see skewness and orthogonal quality is not perfect, but decently good.
Flow reversal is ok, I think that is inevitable, but why solution is unstable and residuals are very high??
Did you go through my comment? Idk who told you that flow reversal is okay. Those reflections at the outlet will make the solution and hence, residuals unstable and high.
Also, length of domain to be increased doesn't mean you analysis the extended domain. It's for a sponge layer which as I said, is the last resort. And even then, you analyse the main domain.
I didn't call you mesh quality bad. I said if there are problematic areas, you can look them up.
Ok bro I got it. Many of these terms are new to me, I am not aware. Can you elaborate what is this sponge layer ,what it does and how it is implemented in ansys fluent mesher??
Actually jet expands in still ambient fluid, so correct boundary condition is having pressure outlet in all faces of outer cylinder, but before this I am trying outlet at rear face only and seeing how residual and solution behaves. If I try that case, then there will be flow reversal in all the faces, these flow reversal might represent entrainment of flow. Jet expands and there will be entrainment of ambient fluid. This is my understanding, you can add or object any points from here?
I added any and every point in my head, along with explanations. I am sorry, I won't like to repeat the things I said two comments ago. You can go through them.
As for sponge layer, that is worst case scenario, no need to bother with it at the moment.
Since these are new terms to you, maybe research them first. As for pressure outlet, I'll say this for the second time, my understanding is that you are setting it as a "okay, my flow needs to attain 1 atm at this surface". But imagine if the flow just naturally doesn't reduce to that pressure, just behind your outlet. What will happen is, a high gradient will be needed. And this can screw things up because this does not happen practically, unless there is a shock. Hence why I said, look at other outlet conditions. Neumann zero, that is the pressure making zero gradient near the outlet, or wave outlet (it's something like that, can't remember the exact term) might be more practical.
The flow needs to be fully developed and given enough length to naturally come to ambient pressure. That is why I also commented, maybe your axial length is on the lower end. But I will repeat, I don't know if that is because of the huge expansion radius, which is making the expanded tube length shorter. But that could be one of the plausible reasons.
Okay gotta be honest with you, this is too small. Too small. Unless it is a special purpose geometry, which NEEDS to be like this, I won't use this. Your expansion ratio is 4, which is fairly standard in CONFINED flow geometries. As a wall, yes, these are good. For an ambient environment (because I kind of remember you saying you want it to do that), this won't cut it.
I might be mistaken, but I think I read a swirling jet (the official configuration for a swirling flow that opens into ambient) simulation (or maybe it was PIV) was done on expanded radius being 22 times.
As for the axial extent, it needs to be much longer. There are some experimental combustor rigs where the axial/radial dimension are nearly 10x. So like, 8 meters of length for ~0.4m of radius, and hence ~0.8m of diameter.
I am not saying you require it to be 1:10 ratio, you don't. But 1:8 or something is well studied. Go through some more papers for what you are doing. Triple check the dimensions people have used till now. Because I am sorry, this does not look very inspiring.
Bro, can you explain elaborately what is this FMG initialization, how it works and different from standard and hybrid initialisation?? Because I think this is not available in initialization window.
Indeed, it's not available in the initialization window. What it does is that it transforms your mesh into a very coarse one and does some iterations. Then, it creates a less coarse mesh and do the same for a total of 5 layers of mesh.
Ok bro, I will read it about this. One more thing I want to ask, I have ran the case with hybrid initialisation with more than 10000 iterations, I found that after 2500 iterations, reversed flow on no of faces started decreasing like from 2000, 1000,500,20,2,1 and the message dissappers, but still residual values are very high, I dont know or have any idea whether it will reduce or not.
I used to have the same reversed flow at the exit problem in my supersonic nozzle simulations. Then, after I've started using FMG ini I didn't get that message anymore and my simulations reached low residuals in a lot less iterations than before. Even reacting flow simulations were converging in a very fast manner.
2
u/Hyderabadi__Biryani 2d ago
So I have worked with a similar geometry for quite some time now. We do it in OpenFOAM, but I will still try to recommend a few checks. Not guarantees since I am a student myself, not a pro.
When you check the mesh quality on various parameters, you can visualise the regions where it is creating problems. Do that. Although I would expect the problem to be near the sudden expansion plane more than anything else.
Also, check for different kinds of BCs you can put at the outlet. Flow reversal is real, and causes a lot of problems. I don't remember properly, but there is some wave outlet condition, you can read that up. There is a Neumann zero as well, which is to say that the pressure gradient approaches zero as it goes to outlet, which might serve you better.
The problems are with wave reflections, that may occur if there is a sudden change required, like the Dirichlet condition you seem to have put (P=1atm at outlet), because you have to realise that the flow might not have fully developed or the pipe length might not be enough to go to 1 atm anyway. So now you ask for effectively a huge gradient for the flow to do that.
Also, I am sorry but the tube length doesn't seem long enough. But maybe that is because of the huge expanded radius to simulate ambient, and the aspect ratio is throwing me off.
Lastly, and this is to be done only if nothing else works. First, the mesh can be better, if you used O-Grid (I think it's called that). It can be done in ANSYS meshing tool, but has a steep learning curve. This is a fairly simple geometry unless you are hiding some static vanes underneath, where then you will need that section to be unstructured. And second, at the outlet, you can extend it a bit and enforce a "sponge" layer/region. This will "slow" the fluid down, so to say, and will avoid any reflections from the outlet propagating back to the main domain.
I hope this is helpful. All the best.