Flow Patterns Randomly Appearing In Transient Sim
 

Good evening CFD-Online,

I am attempting to do some analysis on turbulent flow through a tube with baffling inside. Currently, I am meshing in Salome, and setting my case up in HELYX-OS. My issue is that beyond my inlet, at the first time step, every single baffle produces some sort of velocity. I have attached two pictures. One is at time 0, and one is at the immediate following time step.

Regardless of inlet velocity, or time step, this issue occurs. I have attempted using DES-SA, in pimpleFoam, pisoFoam, and icoFoam, all producing the same issue.

Please let me know what extra information I can provide. Thank you!

-Dan

Well, from the looks of it this is probably a flow feature, so no suprise here. BUT you have to refine your mesh, this is way to coarse for a CFD sim. How many cells do you have?

I made the mesh coarser so I could run variations faster and see if I can solve the issue. Are you saying the coarse mesh is causing this problem? I am currently around 200,000 cells. I intend to be much higher once this is sorted.

Edit: I will go ahead and try a finer mesh before I call it a night

I would not call it an issue, because it's the flow you want to study. Around the baffles velocity must increase because of continuity, therefore you see transient velocity gradients around the edges = vorticies.

In regions with high velocity gradients e.g. your inlet, around the baffles etc. it's good practice to refine the mesh. In other regions it can be coarser.

The continuity is where I have the problem. I have tried making my velocity incredibly small, and my time step incredibly narrow. However, the first instant of the simulation is always flow through the entire tube. Rather than starting at the inlet and marching forward, it immediately goes across the entire tube. It is as if each individual baffle behaves as an inlet.

Also let me thank you for the effort in replying! I hope I can understand this problem soon

Well, this is expected behaviour. I assume you have an incompressible fluid. So the very instant you calculate the flow, meaning the velocity, pressure field etc. so in the very instant of calculation, no matter how small or big the time step is, continuity must be obeyed in every area of the domain. There is nothing which needs to propagate first into the domain. Continuity means velocity increase in area's with small diameter. It's an instantenous effect.

Good luck!

I expect the flow to obey continuity when it reaches the first baffle, however it appears to reach every single baffle and escape the tube at the first time step. I am working on a video that will hopefully highlight the issue better.

My expectations for this simulation were for the flow to begin at the inlet and hit one baffle at a time, and take a given amount of time to exit the tube. Hopefully I can have the video ready soon.

The best example I can come up with is, if you are at a sink: The instant you turn on the sink, the water will work its way down and eventually hit the drain. In my simulation, it is as if the water immediately hits the drain

Ok, try to post the video. Maybe i'm missing something here..

Here is a link to a video.

You'll see a a large amount of velocity initially, then it will diminish at the first time step, and eventually drop to 0 as my simulation ends.
I would expect the flow to begin at the inlet and slowly move over.

No matter what I do, I cannot see the flow propagate through the tube.

Edit: I recommend viewing the video at 0.25x speed

Quick post: it is quite late where I am so I am gonna turn in for the night but I'll be back here tomorrow
I hope I can get this solved soon


Sent from my iPhone using CFD Online Forum mobile app

This yt video is unavaible for me. Black Screen.

I apparently marked it as private on accident. It should be working now. If not, I will reupload tomorrow

Thank you again for your time tonight


Sent from my iPhone using CFD Online Forum mobile app

Ok, can see it now and i see the problem. Was not clear to me from the previous posts. Strange and a bit difficult to tell what the issue here is exactly. It looks like your velocity inlet is temporary or sth.. Can you post BC's?

I'm off now too for a bit..

Flow Patterns Randomly Appearing In Transient Sim
 

For that video, my velocity inlet is time-varying. My intention is to turn the inlet on periodically to see the effect of multiple pulses on a system.



The problem still appears with a contant fixed value velocity. If I make the time step or velocity very small, the animation looks much like the first two image i posted.



Here is a second video with a constant fixed value inlet



For the rest of my boundary conditions, I have a fixed 0 pressure outlet, and everything else is either a symmetry or part of my geometry.

Hi,

have you managed to solve the issue? I just had a look at your second video and i think i know what you mean. I looks like your velocity gradient at the inlet is moving into the domain. Are u sure you have a converged solution for every time step? On the other hand i'm still not sure this is can not be a physical transient effect...

Maybe somebody else with experience can have a look and try to explain.

I haven't solved it just yet.

The residuals look relatively clean. Pressure is a little oscillatory, but I would still call it convergence.

I have a few more things to try and see if I can solve the problem.
Thank you for your effort though!


Sent from my iPhone using CFD Online Forum mobile app

I experimented with boundary conditions and getting rid of some symmetry walls. Still no fix. Hopefully someone can offer some insight

Hi,

@durndurn

Pattern looks like "non-orthogonality induced flow", so, since you have proposed it in the first message, please post the following:

1. checkMesh output.
2. fvSchemes & fvSolution files.
3. your boundary conditions.

checkMesh could be posted inside CODE tags, for other files it would be more convenient if you create archive of fvSchemes, fvSolution files and 0 folder.

Alexey,

The archive is attached and the checkMesh is below.

With 58 degrees of non-orthogonality you can:

- improve your mesh ;)
- use "leastSquares" instead of "Gauss linear" as gradScheme. I.e. fvSchemes file, sections gradSchemes. Do not know why HELYX-OS decided to put "Gauss linear", though it seems Engys guys are not happy with all grad schemes in OpenFOAM.
- use 2 non-orthogonal correctors. fvSolutions, PISO dictionary, nNonOrthogonalCorrectors key.

Start with two last modifications.