Learning Forum

[Daidalos]

Hi i am simulating a transient flow trajectory of a waterjet using the multiphase VOF method with air as primary and water as secondary phase with inlet velocity of 146m/s. attached is an image of my geometry and its boundary conditions. My domain size is 2m wide. however during simulation, i receive reverse flow in my pressure outlet and mass flux inbalance. I believe my domain is sufficiently large so I am not sure why am i receiving this reverse flow. Also, I attached a image of my water vol fraction contour. i do not seem to b e able to see any primary breakup near the nozzle. and after some timesteps, ~1600, the vol fraction does not change much as seen in the below two screenshots. may I have some help regarding this issue?

[Rob]

It looks like the jet is breaking up, and then the mesh isn't well enough resolved to capture the droplets. nBack flow occurs if any flow enters the domain through the outlets: check the flux over the boundary as it could be very small. It's a warning, so unless it effects the solution it's not a problem. n

[Daidalos]

Hi Rob, thanks for you advice, May i ask regarding the mass flux, how do I know if the backflow is affecting my solution. below is the screen shot of my mass imbalance. nnAlso may I ask so the only option for me is to make the mesh finner? since im doing it with a student lisence, I am almost at the element limitations. Is there another way to approachc this issue? I could make my domain smaller but am not sure if that would lead to reverse flow issues affecting my results.nnThanks in advance!nn

[Rob]

The flux balance won't help here, you need to look at the flow field. Does the flow from the boundaries have any impact on the jet, how far from the jet is the flow near enough zero velocity? nRe the mesh. It needs to be finer, so either use a bigger computer (and licence) or consider ways to reduce the domain. Remember we can model sectors rather than the full system. n

[Amine Ben Hadj Ali]

You might think about using VOFTODPM with dynamic mesh adaptation.n

[Daidalos]

Hi Rob, thanks for your advice, From what I interpret from the the velocity contour, the flow from the boundary does not seem to affect the jet. I have split my domain into two and placed a symm BC to reduce the cell count and use it to refine the region of the jet. But not too sure if its fine enough for the given domain. my smallest cell is about 23 micrometers. nnNi DrAmine, thanks for your advice i am trying it now with dynamic mesh adaptation. will post results when done n

[Daidalos]

Hi, sorry i tried to follow this tutorial https://www.youtube.com/watch?v=S0MUu2svgQ8nHowever, after 25 time steps, my simulation stops and does not continue solving after 25 time steps. Been stuck at this for quite a long time. may I know how to address this issue? thanksnn

[Rob]

How many cells have you got at 24 time steps? What's the RAM & cpu load at when it's stuck?n

[Daidalos]

nHi Rob, thanks for the quick reply, attached is the CPU and ram usage when its stuck. CPU usage turns 0. Not sure how to check the cell count when the iteration is frozen at the 25 time steps, but the initial cell count is approximately 480k. Just wondereing does it have to do with me using a student version with a limited cell count of 512K? n

[Rob]

I'm wondering that, it wouldn't take much adaption to push you over the limit. With 30k cells spare you'd only need to adapt about 4k cells to hit the limit. The lack of cpu suggests that something is stuck, if the solver was trying to do something at least one cpu would be at 100%.n

[Daidalos]

So dynamic mesh adaptation is still limited by the 512K cell limit? And the solver is stuck as I might have exceeded the cell count during the dynamic mesh adaptation. If so I think dynamic mesh adaptation would not be a solution for me. would it help if I start with a much coarser mesh before adaptation? n

[Daidalos]

I tried duplicating the workbench after removing the dynamic adaptation, then re-initializing and reapplying dynamic adaptation. I increased the time step slightly to 3e-7 from 2e-7. Currently the iteration just went pass the 25 time step mark. but CPU usage is still extremely low (0.1%) for the solver. I Hopefully the simulation manage to completen

[Daidalos]

Hi, may i ask to check my boundary conditions? I think I have the right boundary conditions set. but jsut want to double check if its not an issue with my boundary conditions. Regarding the reverse flow at pressure outlet, I think the issue might be due to bad mesh transition. as shown below. Might that be the problem? Have checked my skewness/orthogonal quality and aspect ratio, everything is below the recommended limits. I read that reverse flow doesnt affect solution and may wither away after iterations and that it affects the convergence. My reverse flow faces only seem to be increasing in the number of faces.pressure outlet (gauge pressure =0) operating pressure = atm (101325Pa)nnsymm BCnBottom wall (no slip) - impact wallntop wall (physically would be atmospheric, but I cant use outlet pressure since it is too close to the nozzle inlet. nnozzle inlet BC (velocity 150m/s VF =1)nbad mesh transition?? n

[Rob]

It's not great but assuming the jet is in the middle it's fine. I'd significantly reduce the domain extents and also reduce the aspect ratio in the jet region. Think how the jet interacts with the moving liquid: ie how the front of the jet moves through the cells. Re the domain extent, if you run a tap how far away from the water would you need to measure experimentally? n