[aipatel]

I am trying to model a separator that draws in a mixture of fluid and air due to a vacuum pump. Air exits through one pipe and the water exits through another pipe.

There are two baffles between the inlet and air outlet pipe in order to stop any water from flowing through that outlet. As of right now, I have specified a fluid dependent mass flow at the air outlet of only air and 0 water, and have a fluid dependent mass flow at the water outlet of only water and 0 air. And a total pressure at the inlet I calculated using velocities I calculated since I know the mass flow as well as the volume fraction.

I have a few problems, the solution diverges eventually (after a few hundred iterations) which I think is a mesh problem so I am currently remeshing with a finer mesh density. But I took a look at the intermediate unconverged results. I plotted water velocity backwards from the air outlet and there are streamlines, which doesn't make any sense since when I plot the volume fraction, there is no water in that area. The imbalances are also quite high for the water on the order of 30% before it diverges and crashes.

I have tried solving only air with a stationary water column and using that unconverged solution (imbalances were <0.01 %) and using that as initial conditions when I add water into the problem. I know multiphase flows may not converge at steady state, but I at least need something reasonable to start a transient solution with.

I was wondering if anyone had any insite? Any help would be greatly appreciated.

[ghorrocks]

I think is a mesh problem so I am currently remeshing with a finer mesh density.

A finer mesh is likely to make it worse, not better. Finer meshes have less numerical dissipation and therefore higher numerical instability. You have a numerical instability problem. See FAQ: http://www.cfd-online.com/Wiki/Ansys...do_about_it.3F

If this simulation runs for a while then diverges then something is probably happening to cause the divergence. Have a look in the post processor for something happening int he flow like some water reaching an outlet or a chamber filling up or a duct being blocked.

[aipatel]

Thanks for the response.
Oh I see, I will focus on a coarser mesh but with a thick inflation layer.
The simulation diverges soon after water hits the floor and starts to splash upwards, at least that's how it looks in the post processor. Pressure values also skyrocket at the points where the water hits the floor perpendicularly because the outlet pipe is not directly under the inlet. I have tried curving the bottom floor surface, but that did not seem to help.

[ghorrocks]

You should only use coarse meshes for developing the model. You are going to need to run fine meshes soon enough. To improve the numerical stability the most important thing is mesh quality.

It looks like you have found the thing causing the problem (water hits the floor). I would consider setting small time steps in this phase. Alternately use adaptive time stepping homing in on 3-5 coeff loops per iteration and it will do it automatically.

[aipatel]

I've been trying to get a steady state simulation that looks okay to start a transient simulation from. Do you think letting the steady state simulation run for only a short while then starting up the transient from that is a valid approach?

[ghorrocks]

Yes, if you do not care about the startup transient.

[aipatel]

Glenn,

I've run a test model without any complicated geometry and it seems splashing is the issue that is causing the divergence for the steady state analysis. I am using a timestep of 0.001s initially and it seems that is too large for the splashing. Tank is about 2 m high and inlet velocities are on the order of 10 m/s. I am wary of running transient because of how long it will take to run. I asked a coworker about the problem and he thinks that running this model steady state might not be doable with the amount of splashing involved.

I wanted to know if you have any insight into the splashing problem or if a smaller timestep during that phase will fix the problem. I assume mesh quality would also cause the solution to diverge during the splashing correct?

[ghorrocks]

Free surface simulations frequently need to be run transient to get convergence, and that is when they appear steady. If you know you have transient features (ie splashing) then you certainly will need a transient model.

[aipatel]

Glenn,

Thanks for your help. I will run this transient, with a larger time step until water hits the floor then a smaller one after that. I am running a comparable test model (one without so many walls) and it seems to be fine, just extremely slow.

[aipatel]

The simulation diverged. It seems to be mesh quality as this point, I am wary of going lower than 1e-5 s for a timestep. I have a very thick inflation layer of mesh, a few inches. I read that for accurate surface tension modeling the aspect ratio should be <= 1.5 unless the element is long the flow direction. For splashing on the floor this would not be the case. I was wondering if you agreed with this.

[JuPa]

Switch off surface tension. Does your simulation work without it?

[ghorrocks]

If you are modelling this with surface tension then everything changes:

I am wary of going lower than 1e-5 s for a timestep

Bad move. Surface tension needs very small timesteps. If it needs smaller time steps then let it.

I read that for accurate surface tension modeling the aspect ratio should be <= 1.5 unless the element is long the flow direction.

For accurate surface tension modelling you need hex meshes with aspect ratio <1.2. You cannot do accurate surface tension modelling on a tet/pyramid/inflation mesh. And there is no exception for the flow direction, you cannot exceed it in the flow direction either.

[aipatel]

I have turned off surface tension and that helped a ton. I misread the FAQ on the aspect ratio needed for surface tension. It also allows the use of a larger timestep which means faster run time.

Now the only problem I still have is the water velocity streamlines forwards from the inlet is going to the air outlet instead of the water outlet. This happens at the first time step. And starts changing as the solution progresses. Streamlines forwards from the inlet seem fine though.

I have set water velocity components to 0 as an initialization of the domain. So I am not sure why this is occurring. My only guess is how I set my boundary conditions. Mass flow inlet of both air and water. Mass flow outlet of air and 0 water and opening static pressure for the pipe that empties the water.

But other than that I think I have it under control now. Thanks a lot for your time and help.

[ghorrocks]

If surface tension is important in the physics then you have to turn it on. For instance droplet formation will require surface tension. But if it is not important you must turn it off because it is a very expensive model to use and will make the simulation much more difficult.

[aipatel]

Ah okay, effects like droplet formation are not important in this model.
I am currently running a small section of the main model transient and it is running well.

[aipatel]

I've had a decent amount of success with the model after looking at my mesh in detail and seeing i had some really skewed elements.

I have changed the CFD mesh to better represent the actual geometry. I have an inlet pipe directing water towards a vertical wall at a ~45 degree angle. In this tank, we are concerned with splash back from the walls.
In my models, I am seeing any water basically sticking to the walls and falling straight down. Any splashing that occurs is water on water interaction and not water on wall interaction.

I am currently using the free surface, continuous model for both air and water, but with surface tension off and drag coefficient set at the default 0.44.

Any insight would be helpful, thanks.

[bshkoj]

Hi. can every one help?
I want to simulate water surface profile over weir using ansys cfx code and i used RNG turbulence model. but the results are not good and i can not get the ventilation region in water profile. and i don't know to determine water surface profile (polyline) at center of channel.

[ghorrocks]

FAQ: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F