Domain Reference Pressure and mass flow inlet boundary
hello everyone, im very stuck with the settings of my boundary condition and specially with the referente pressure:
im modelling combustion with flamelet, and i want to use mass flow for all the inlet (air and fuel), the air enters to the chamber with 6.4bar and the fuel with 14.31bar, my question is: how can i set the mass flow boundary for a specific pressure? when i set this boundary, i just set the temperature, but the density depends on pressure and temperature, how can i set this two different mass flow? another thing its, the domain reference pressure affect to the whole domain, so, if a set the boundary of fuel (mass flow) this mas flow will be affected for this pressure, so im not sure to what refference pressure set.(i was using the pressure of the inlet air, becuase in a chamber its relleativy constant). well, please helpe im vvvvvvvvvery stuck with this thanks ver much 
If you know both the mass flow rates and pressures of the input gases then I would use a mass flow rate boundary for the inlets and a pressure boundary at the outlet (I assume you know the exit pressure  it is probably just atmospheric pressure with a small allowance for exhaust pipe losses). Then you can check the input gas pressure as a check of the accuracy of your simulation.
The reference pressure is purely a numerical thing. You set the reference pressure so the numerical accuracy of the pressure field is higher as the solver works on the pressure relative to the reference pressure. Set the reference pressure to be the outlet pressure (if you are using a pressure outlet) or the average pressure in the chamber. The exact value you use is not really important, but you do need to make sure all pressures you specify are correct relative to the reference pressure. 
Thanks very much for your time:
First: im trying to use inlets mass flow boundary because i read in some pdf, that's is a better choice for compressible flows instead of velocity im a right?. second: in a firts time i was using the tutorial of combustion, for the setting of the reference pressure (1atm) and pressure boundary outlet (0Pa). but this is correct? 0Pa to the outlet its a very very low pressure?, in my case i dont have any information of the pressure outelet, so im using this configuration: 6.40(bar)>reference pressure (this value its the pressure of the inlet of air) 6(bar)> to the oulet boundary condition (because in a combustion chamber of a turbine, generally the losses are of arround a 6%). but im not sure if this its right?, in this moment, i just want to make an a firts aproximation of this simulation, and im wondering who value is the better choice, the values of the tutorial (for reference 1atm and outlet pressure 0Pa),or mines =/. another things its, when i run the simulation with velocitys, the flow field(temperature,radiation) are not homogeneous, and all the boundary has the same value, like this image (when i try with randoms values of mass flow rate boundary, this not happend):(the first image its the good one =) ) http://img194.imageshack.us/img194/1120/finalzw.jpg http://img189.imageshack.us/img189/5457/98398525.png sorry for all the inappropriate question but im working by myself in CFD, and i dont have anyone to ask about the settings of the software =/. thanks very much for your time best regards Mauricio:D 
Quote:
ohh and i forgot,my values of mas flow rate are in the ISO CONDITION (15ºc and 1atm)(from the documentation of the turbine), but in the operation of the turbine i have other values for temp and pressure, what can i do? 
You cannot set both the flow rate and pressure at the same boundary. It is a numerical impossibility. Do some reading on "well posed boundary conditions" for CFD simulations.
It should be a trivial matter for you to convert the flow rates at ISO conditions to any other temperature and pressure. If you can't do this then why are you doing CFD? .......and anyway, if you know the mass flow rate it does not matter what temperature and pressure you are at! 
you have rigth,
im gona check if this boundary conditions are correct. thanks 
if you know the inlet mass flow rate and pressure value, you are lucky, because if you set the mass flow after the simulation you can check the pressure at the inlet, and you can validate! setting both value means an overconstrainted boundary contition, where you set two quantities wich depend on each other.

Attesz:
thanks very much for your reply, im working wiht approximate mass flow rate for the inlet boundary, what do you recommend me for the outlet? pressure o mass flow rate? (the pressure outlet its an aproximation to, i dont have the exact value). thanks 
As I said, it looks like you need to do some reading into well posed boundary conditions. Some combinations of boundary conditions are not possible and will never converge. Mass flow rate inlet and mass flow rate outlet on a steady state simulation is an example of an impossible boundary condition. The documentation has some basic information about this, I think under choice of boundary conditions.

yeah, you have all right, in the documentation said:
best robustness: mass flow rate or velocity (inlet) and for oultet:pressure im using for the outlet static average pressure. but its true that for compressible flows (combustion case) its better use mass flow rate for inlet boundary instead velocity?. thanks 
mass flow rate or velocity inlet are good, static pressure outlet also. i recommend not to use averaging, because the solver use that value for the whole area, and can give bad results.
i dont know, how disturbed is the flow at inlet and at the outlet. if the inlet flow is consistent, and the outlet not, maybe inlet total pressure and outlet mass flow is better, because the pressure at outlet is very uneven. you must set boundary conditions taking into account the real phenomenons... 
thanks very much for your reply :)
yeah one of my difficults its the exact value for the inlet or outlet boundary, because this turbine(hitachi ge frame V 1974) its very old and dont have measure instrument in the places that i need ( mass flow of air, temperature of combustor) so im using aproximation based on tables parameter of the turbine. it was very helpful, im gonna use your advice for the outlet pressure, im gona use just static pressure and not the average static pressure. thanks very much:) 
ghorrocks; sorry for that stupid question about the mass flow rate boundary! i really dont know what i was thinking:rolleyes:. my simulation finally walk well. when i use 0bar for reference pressure and some static pressure for the outlet everything works fine, and the results inlete velocity correct.
thanks very much again, and sorry for that stupid question :D, the first think that imgona do finishing this work, its sleep long time! best regards 
Quote:
Could you please explain why do you say that? I am confused. If you have a pipe which branches into two. I set a mass flow inlet and then put say 30% of mass flow outlet in one branch and 70% in another. For incompressible steady simulation, why is this wrong? 
It cannot work because there is nothing to define the pressure.

Quote:
I still agree that theoretically only one node pressure value is sufficient to solve all mass flow BC case. 
You are correct. It does mean the absolute value of the pressure is arbitrary. So I move onto the second problem....
If you define the mass flow rate in and out of a domain in a steady state simulation, then it is not possible to achieve imbalances convergence. All floating point numbers are approximate in a computer, meaning that after floating point approximation your inlet flow will not balance your outlet flow. This small imbalance in flow rates cannot be removed as there is nothing the solver can adjust to balance it. This means you cannot converge the imbalances in this approach. This imbalance may be small or large depending on your simulation setup. More completely: Your simulation is not well posed. Wikipedia's definition of well posed (https://en.wikipedia.org/wiki/Wellposed_problem) states that the solution has to be unique. Your condition with the boundary conditions only is not unique as the pressure level is not set, and therefore is badly posed. You have to make an additional assumption of the pressure at a point to make it solvable. Here is another reference which dives into more mathematical rigour on the definition of well posed: http://liu.divaportal.org/smash/get...FULLTEXT01.pdf 
All times are GMT 4. The time now is 01:04. 