[Mariana Marin]

Hi, I am currently running my simulation of a transient liquid flow through a flow separator structure (excess flow spills out and the other continues down the pipe). according to the previous forum published ([URL="http://https://forums.autodesk.com/t5/cfd-forum/convergence-plot-interpretation/m-p/11933470#M30051"]) my simulation has already entered a state of total convergence of the transient variables, but when measuring the volume flow rate in the outlet pipe, it decreases as it progresses through the pipe, as follows:



In the inlet pipe (red) the stability of the volume flow rate is observed, but in the outlet pipe (yellow) despite the fact that the variables converge, this decrease and variation in the volume flow rate continues.


* The only BC that the model has are volume flow rate in the initial face of the inlet pipe and pressure = 0 in the 3 outlets of the flow.

* The model with denser meshes (smaller element size) has already been simulated, but this problem continues to occur.

* the time step size satisfies Courant's law.

* the model is run in a transitory state and with 3 inner iterations.

* The slope of all geometry is equal to zero.

* The volume flow rate was measured with planes at different points of the outlet pipe with the help of the bulk tool:



I am open to any suggestions, big or small, on how I can achieve volume flow rate stability in the outlet pipe.

You can see the complete forum in the following link:https://forums.autodesk.com/t5/cfd-f.../td-p/11952548

[arjun]

" the model is run in a transitory state and with 3 inner iterations."


increase this number. Also solve the continuity to tighter tolerance. Continuity plays important role in mass loss.

Unfortunately losing the mass in VOF calculation happens and it is solver based. Pretty much all solvers lose to some extent. The only solver where I know that this issue is properly addressed is the one I write ie Wildkatze. Here we created specially procedure to ensure mass balance after every time step. I am not aware of such procedure in any other solver.

[JBeilke]

Setting p=0 at the outlet of the horizontal pipe is one of your problems. You have to specify a linear pressure increase from top to bottom according to the level of water. Otherwise the water will flow out faster than expected in the lower part of the pipe and a backflow of gas will happen in the upper pipe. Your picture looks like this.


Last time I worked on such a problem I used an "Outlet" instead of "pressure outlet" in StarCCM+, which worked very well.