[Bdew8556]

Hey guys,

Just looking to do a deep dive into why we use pressure or density based solvers for different applications and how that affects our domain size.

Solvers:
To my knowledge pressure based solvers are used for low speed flows because density does not change (very small changes). pressure based solvers can be sequential or coupled, coupled being the SIMPLE algorithm and it's various cousins?

Far field conditions:
We can use far field conditions with the pressure based solver but they must be a certain distance from the object. In an aviation setting this is usually an aircraft where you set the domain size to be x 10, x 20 aircraft length away from the aircraft. this is to make sure there isn't a mach change at the boundary yes?
Does this mean the far field condition varies pressure and velocity in order to achieve a constant mach? I hear all this stuff about the reimann variable but nobody seems to know exactly what that means.

Density based solver:
However with density based solvers for high mach flows, eg a missile on re entry, I've seen people use very small domains. Is this because the density based solver can handle shock waves at the far field boundary? ie it can calculate density explicitly so having a mach gradient at the boundary isn't an issue?

Just trying to understand this from a 'gut' level if that makes sense.
Oh and I swear to god if someone comments "read the manual", yeah.... you're not clever bro.

[sbaffini]

You have, in your mind, a collection of completely random facts which are not true. How can we even remotely be assumed to be able to change that in a post or two? We can't.

So, from the gut, read an effing book bro

[Bdew8556]

How are they not true? do high speed density based simulations not sometimes use boundaries close to the object? why is that ok with density based solvers but seemingly not pressure based solvers?

[FMDenaro]

Originally Posted by Bdew8556

How are they not true? do high speed density based simulations not sometimes use boundaries close to the object? why is that ok with density based solvers but seemingly not pressure based solvers?

Who told that? Have you read this statement in a CFD textbook?

[Bdew8556]

I've seen work/papers setup like this. Maybe those works were doing something wrong? quite possibly, it jumped out at me that it was odd and the only difference was the pressure v density based solver.

[FMDenaro]

Originally Posted by Bdew8556

I've seen work/papers setup like this. Maybe those works were doing something wrong? quite possibly, it jumped out at me that it was odd and the only difference was the pressure v density based solver.

Pressure or density based solvers have nothing to do with the theoretical extension of the domain and location of boundaries. These latter depend on physical considerations about the influence of the numerical BCs.
Could you post the papers you have read?

[Bdew8556]

Cool, that helps answer my question. I'll have a look to see if I can find the specific paper I recall. Did some quick googling and found this:
https://www.ata-e.com/software/train...-dynamics-cfd/

Any difference in the way pressure v density solvers interact with the far field condition? sounds like its the same?

[sbaffini]

Let's see...

SOLVERS: since more than 20 years pressure based solvers in commercial CFD codes can be used for variable density flows, including highly compressible ones, and have no specific limitations with respect to density based solvers. It is true that pressure based solvers can be either SEGREGATED or coupled, but SIMPLE family, PISO family and other fractional steps solvers are all segregated. There are a few coupled pressure based implementations out there, but none of the authors cared about naming them (to the best of my knowledge), so what people usually mean when talking about a pressure based coupled solver is, in fact, the one implemented in their CFD code of choice.

Modern implementations of density based solvers also bypass their major limitations trough preconditioning and dual time step.

All in all, it obviously makes sense to use pressure based for low to non compressible flows and density based for highly compressible flows. But it is more a matter of efficiency than anything else.

FAR FIELD BC: The FLUENT bc called "pressure far field", which is a totally arbitrary naming convention, is based on preserving/extrapolating the Riemann invariants for the ingoing and outgoing waves and is based on an ideal gas assumption. If your scheme is an approximate Riemann solver or similar (and it sort of must be in order to work with compressible flows) then using your scheme at the boundary is pretty much the same concept. In any case, Mach number is not an invariant and it will vary with all the other variables. What is pretty much accurate in the naming is that FAR FIELD, as most bcs, is meant to be put on a... far field. The only case where disturbances won't affect the close boundary is, schematically, for fully supersonic inlets BUT... this must be steady and you have to get there starting from your initial solution. Every other use case is misuse and, unless confirmed to be ininfluent trough tests, has a misplaced boundary.

SHOCKS AT BOUNDARIES: every working compressible code must be able to handle shockwaves passing trough boundaries. Still, the limited/inaccurate informations we have at open boundaries, in addition to the further approximations we introduce in the discretization there, make them a zone that is always better put away from your zone of interest, no matter what.

[FMDenaro]

Originally Posted by Bdew8556

Cool, that helps answer my question. I'll have a look to see if I can find the specific paper I recall. Did some quick googling and found this:
https://www.ata-e.com/software/train...-dynamics-cfd/

Any difference in the way pressure v density solvers interact with the far field condition? sounds like its the same?

I don't see something relevant to the discussion about BCs. Clearly, density-based formulation is suitable for high compressible flows.
Hypersonic flows is complex due to ionization, dissociation, eventually also due to lack in the continuum model.
You should check the topic in well known textbook, not in industry presentation.