Thx KAKM for the fruitful discussion. Cfdof gives the abiltiy to define a boundary as "constraint" - symmetry of flow quantities about boundary face.
What kind of boundary is that specifically ? Does it mean for example that any flow normal to the boundary face has a counterpart poniting in a
oposite dirtection ? Or how can I imagine that ?
Or let me ask in oter words: if you have a free water surface (as the most up face of my tank model is) whcih boundary condition would be the most
suitable ?
Question to convergence and residuals
Moderator: oliveroxtoby
Forum rules
and Helpful information for the FEM forum
and Helpful information for the FEM forum
-
- Posts: 114
- Joined: Wed Apr 17, 2019 2:08 pm
Re: Question to convergence and residuals
A symmetry boundary condition has no flow across the boundary. It's used for things like an airplane flying straight–the flow should be identical (mirrored) on the left and right half of the airplane, so it doesn't make sense to model all of it. Instead, you can cut the airplane down its length, put a symmetry boundary condition on the cut part, and get equally good flow results using half as many cells.
Well, if you care about what the free surface is doing you should use an two-phase/multiphase solver like interfoam and put the boundaries away from the surface. If you just care about what's happening in the tank well below the surface, you can make the top of the tank an outlet (pressure outlet at atmospheric pressure would probably make sense) or an open boundary condition at the top, which would essentially imply an arbitrarily large fluid region on the far side of the boundary and that the fluid keeps doing whatever it's doing right before the boundary. Be aware that flow right next to the outlet might be a bit funky, especially if there's backflow through the boundary. So I guess the most accurate answer (as it often is in CFD) is that it depends on what information you're trying to get out of your simulation.
Well, if you care about what the free surface is doing you should use an two-phase/multiphase solver like interfoam and put the boundaries away from the surface. If you just care about what's happening in the tank well below the surface, you can make the top of the tank an outlet (pressure outlet at atmospheric pressure would probably make sense) or an open boundary condition at the top, which would essentially imply an arbitrarily large fluid region on the far side of the boundary and that the fluid keeps doing whatever it's doing right before the boundary. Be aware that flow right next to the outlet might be a bit funky, especially if there's backflow through the boundary. So I guess the most accurate answer (as it often is in CFD) is that it depends on what information you're trying to get out of your simulation.
-
- Posts: 114
- Joined: Wed Apr 17, 2019 2:08 pm
Re: Question to convergence and residuals
Mainly i am interested in what s going on in the tank not so much about the currents directly on the surface. So, for this issue you would recommend an open boundary or a oulet with pressure definition. I'll try.
Re: Question to convergence and residuals
I'd suggest the pressure outlet. I think there may be stability issues with the open boundary–I don't think it bounds pressure, and that wouldn't play well with a velocity inlet.
-
- Posts: 114
- Joined: Wed Apr 17, 2019 2:08 pm
Re: Question to convergence and residuals
Currently the sim is running with the surface defined as pressure outlet. What I note up to now is that the pressure residuals do hardly dive below 10^-2. Velocities and turbulence energy goes down to a high 10^-4. Turbulence dissipation dive down to 10^-5.
What would you say about this behavior ? The pressure residuals semm to me quie high.
What would you say about this behavior ? The pressure residuals semm to me quie high.
Re: Question to convergence and residuals
What the residual is doing matters more than the absolute value. If that's the value the pressure residual started at, you might have a problem, but if there has been a roughly asymptotic decrease, it's probably not an issue. If there's a strongly cyclic element, then there's likely some periodic behavior in your system. I'd suggest taking a look at your solved pressure values and see if they make sense–residuals are not the end-all, be-all for whether a simulation has properly converged/given reasonable outputs.