[giulypa_1985]

what is the difference between the "pressure-based solver" and the "density-based solver"?

[Galileo]

I am not sure you are a biginner in Fluent (like me), but I think it might help to ask which Solver is better for your problem and why?

Going through the Fluent Manual, there are a lot of differences and depending on what you are solving. Unless your question is enumerating the differences, I think you may want to ask that question based on your problem type, for example Density Based solver is not available for Eulerian multiphase model framework, you will use the pressure based solver. You can do stuffs like solidification and melting model only with PBS.

The PBS is said to employ a projection method algorithm, in this algorithm, mass conservation of the velocity field is obtained by solving a pressure/pressure correction equation in a way to satisty the continuity iteratively till convergence.

The DBS attempts to solve the Continuity, Momentum, Energy and Transport eqns. in a coupled manner i.e. simulataneously. then followed by additional scalar transport equation.

Some solution schemes may be available in PBS and not in DBS e.g. Central Diff. Scheme (CDS)., Bounded CDS.

For your PBS, you can use (generally): the following pressure-velocity coupling algorithms:
SIMPLE,SIMPLEC, PISO, Coupled and Fractional Step.

Note also that PBS allows both Coupled and Segregated options.

Hope this helps and not confusing

[giulypa_1985]

i'm using fluent for modeling the dispersion of methane in air. the methane is introduced in air at 111K. I don't konw if is better use the density-based or the pressure-based models in the calculus.

[Galileo]

Originally Posted by giulypa_1985

i'm using fluent for modeling the dispersion of methane in air. the methane is introduced in air at 111K. I don't konw if is better use the density-based or the pressure-based models in the calculus.

Sourced from:FIT Material

The following features are available with the density-based solver, but not with the pressure-based solver:
These are the "only" features available with the Density Based Solver:
1. **Real Gas Models (UDF and NIST)
2. Non-Reflecting BC
3. Wet-Steam Multiphase Model

Otherwise (as in your case), you may want to use Pressure Based Solver.

PBS is available for:
Cavitation Model
Volume-of-Fluid (VOF) Model
***Multiphase Mixture Model***
Eulerian multiphase model
Non-Premixed Combustion Model
Premixed Combustion Model
Partially Premixed Combustion Model
Composition PDF transport Model
Soot Model
Rosseland Radiation Model
Melting/Solidification Model
Shell Conduction Model
Floating Operating Pressure
Fixed Variable Option
Physical Velocity Formulation for Porous Media
Specified Mass flow rate for Stream-Wise Periodic flow

The coloured/asterisked options above look to me like what you are trying to do.
You may do a trial run on DBS to compare anyway.

[mohsen tavakol]

hello
i want to simulate a supersonic multi phase flow in fluent.
the phase are air and steam as ideal gas.
as i know, for simulating supersonic flows, we should use density based solver. but multi phase is disable in density based solver.
please guid me.
thanks.

[uday sarkar]

Hello
simulating supersonic flow and combustion together seems not possible with density based solver so is it ok to go ahead with pressure based solver?
Can anyone help?
Thanks

[utsavac]

Uday,

Maybe its too late to answer but I wouldn't use pressure based solver for compressible flow problems (supersonic). Though density based solver can be used for both compressible and in-compressible solutions, I have seen that pressure based solver performs poorly for compressible problems. I hope this helps. When I do in-compressible combustion, I use pressure-based solver with coupled algorithm.

[dequick.b@gmail.com]

Originally Posted by uday sarkar

Hello
simulating supersonic flow and combustion together seems not possible with density based solver so is it ok to go ahead with pressure based solver?
Can anyone help?
Thanks

I have the same problem... I want to model a rocket combustion chamber (with separate oxidizer and fuel inlets), followed downstream by a CD nozzle. As from the throat section, the flow becomes supersonic. But non-premixed combustion model is only available with pressure based solver (not suitable for supersonic flow).

Anyone an idea on how to proceed? Thank you!

[LuckyTran]

Originally Posted by dequick.b@gmail.com

I have the same problem... I want to model a rocket combustion chamber (with separate oxidizer and fuel inlets), followed downstream by a CD nozzle. As from the throat section, the flow becomes supersonic. But non-premixed combustion model is only available with pressure based solver (not suitable for supersonic flow).

Anyone an idea on how to proceed? Thank you!

What's wrong with the pressure based solver? It works for supersonic flow.

[dequick.b@gmail.com]

Originally Posted by LuckyTran

What's wrong with the pressure based solver? It works for supersonic flow.

Thanks LuckyTran! That would be great. I've read in some places that the pressure based solver is not suitable for supersonic flows (inaccurate). I must admit I don't find anything about this in the user manual though, but I just wanted to be sure.