Are you using turbulence scheme ?

hey btw

If I recal for LES I think I saw somewhere in tutorials from Jozsef Nagy (or someone else) that usually you don't want to have Co > 0.7

Either way for turbulence I think it was around 1 and 2 max for some simulation. I am outta work now but I can have a look at it tomorrow morning if you are interested

Its RANS, k epsilon standard...

Yeah okay. I'll stay conservative at 0.8 for now, coz this is a lonnng sim and the only priority above speed is that the solution shouldn't turn out totally crap.

So after asking my seniors, ideal is 0.5 for RANS and never above 1

(my group works in thermodynamics applied in water boiling)

I'm now at Co=0.3 😬 although a completely different case

So just my 50cts that I would not trust at all. Basically each time we solve an equation in OpenFOAM we implicitly solve a linearised version of that equation. This means that to deal with the nonlinearity of the equation we must repeat this process multiply times, and with each repitition the temporal "solution" behaviour of our solver gets closer to a "truly non linear euler implicit" solver. Which is unconditionaly stable.

Now stable is very far away from accurate. Euler implicit is only accurate for processes that are "slow" with regards to its timestep. Thats why to get accurate results you must have a low Courant Number, whereas when just stability is a concern you can crank up the corrector steps, and take advantage of the high stability.

Since you mentioned being afraid of creating an unphysical solution by running with a high co number at first, from which you cant recover afterwards even if you lower the co number I would argue, that this risk allways exists. Since your initial guess is most likley a unphysical one. We most allways assume that the solver will converge to a physical solution even when starting with a unphysical one therefore Id say starting with a large timestep, even though that will lead to fast processes being way to strongly dampened is not a problem.

Yeah I just need to get past the initial transient phase even it is not very physical in that period. But I'm not sure if I should do a Co>1 in multiphase as the interface may begin to fly off into oblivion.

I fear that is case dependent but of cause with keeping it low your on the safe side

not a multiphase expert, but could it help to use local time stepping?

No unfortunately I don't think this aligns with my use case.

First simulate with a coarse mesh, and then map the solution to fine mesh and continue

I really appreciate the suggestion 🙂 I wish I could do that - its an annular pipe with core of one phase and annulus of another, so I cannot do without a certain resolution - I do have super-coarse mesh everywhere that I could afford (everywhere away from the region of interest - after having convinced myself that solution remains largely unaffected by super coarse away mesh) I did think of breaking it down into AMI type two domains, generating one part the problematic annulus by itself to steadiness and then using its surface as an interface with downstream part to develop it separately. But unfortunately I don't have so much time to experiment with these tools at the moment so I'm just brute forcing through the whole domain. Unfortunately it comes with the cost of time, as may be expected.

@qr I agree with this if I’m interpreting it right. In my experience I use high courant to get quicker convergence and then run final , solution with lower courant or different schemes and turbulence models and then the final solution matches physical modeling very well. This is in models with pretty high Reynolds # though where inertial forces dominate

I got a case with fixed pressure values on both the inlet and outlet, what bondary condition should i use for the U field in the inlet? The idea is to get the flow rate as a result. The volume is nothing crazy, a straight pipe basically

For some reason nothing i found online seems to converge

I'd imagine that fixing pressure gradient automatically result in flow? Something like Bernoulli at least as a lump sum non turbulent mean flow?

Does it converge for small difference but not for larger ones? (That maybe caused due to flow instabilities)

Imo the main problem ist that this combination of bcs results in a very bad initial guess if you use a uniform internal pressure field

Basically what you are starting out with is a shock tube due to the local jump in pressure you have at either inlet or outlet

Resulting either in a shock traveling down stream or a „dilution wave?“ (germans call it a verdünnungsfächer) traveling upstream

Both lead to large local gradients which you will not be resolving (would make no sense for the steady state result) resulting in well problems due to the unresolved non linearity

Furthermore even if you get the thing stabil enough (lots of artificially dissipation id guess) to get the right result you will have to iterate till those shocks decay because they get reflected at your domain boundaries

What id try is starting of the simulation with a linearly decaying flow field, or try the standard setup where you fix velocity at the inlet instead of pressure and use a programmed boundary condition that samples the inlet pressure and calibrates the velocity till you reach your wanted pressure drop

You could try [totelPressure ](https://doc.openfoam.com/2306/tools/processing/boundary-conditions/rtm/derived/inletOutlet/totalPressure/) for p and [pressureInletOutletVelocity](https://doc.openfoam.com/2312/tools/processing/boundary-conditions/rtm/derived/inletOutlet/pressureInletOutletVelocity/) for U on inlet and outlet. I had success with this in a similar case.