# Domain Reference Pressure and mass flow inlet boundary

 Register Blogs Members List Search Today's Posts Mark Forums Read

 January 19, 2010, 20:29 Domain Reference Pressure and mass flow inlet boundary #1 Member     Mauricio Caamaño Flores Join Date: May 2009 Location: Punta Arenas, Chile Posts: 62 Rep Power: 9 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

 January 20, 2010, 17:07 #2 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 12,638 Rep Power: 98 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.

 January 20, 2010, 23:15 #3 Member     Mauricio Caamaño Flores Join Date: May 2009 Location: Punta Arenas, Chile Posts: 62 Rep Power: 9 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 =) ) 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

January 21, 2010, 01:15
#4
Member

Mauricio Caamaño Flores
Join Date: May 2009
Location: Punta Arenas, Chile
Posts: 62
Rep Power: 9
Quote:
 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 really know the mass flow rate, im ok with that, but, how can i set the pressure inlets for that mass flow rate? in the setting of the inlet boundary mass flow rate just ask for the temperature. how can i set for inlet boundary mass flow rate with pressure?

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?

 January 21, 2010, 17:42 #5 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 12,638 Rep Power: 98 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!

 January 21, 2010, 19:57 #6 Member     Mauricio Caamaño Flores Join Date: May 2009 Location: Punta Arenas, Chile Posts: 62 Rep Power: 9 you have rigth, im gona check if this boundary conditions are correct. thanks

 January 22, 2010, 04:00 #7 Senior Member     Attesz Join Date: Mar 2009 Posts: 355 Rep Power: 9 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.

 January 23, 2010, 01:20 #8 Member     Mauricio Caamaño Flores Join Date: May 2009 Location: Punta Arenas, Chile Posts: 62 Rep Power: 9 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

 January 23, 2010, 02:07 #9 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 12,638 Rep Power: 98 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.

 January 23, 2010, 02:54 #10 Member     Mauricio Caamaño Flores Join Date: May 2009 Location: Punta Arenas, Chile Posts: 62 Rep Power: 9 yeah, you have all right, in the documentation said: best robustness: mass flow rate or velocity (inlet) and for oultetressure 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

 January 23, 2010, 05:12 #11 Senior Member     Attesz Join Date: Mar 2009 Posts: 355 Rep Power: 9 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...

 January 23, 2010, 06:00 #12 Member     Mauricio Caamaño Flores Join Date: May 2009 Location: Punta Arenas, Chile Posts: 62 Rep Power: 9 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

 February 11, 2010, 21:28 #13 Member     Mauricio Caamaño Flores Join Date: May 2009 Location: Punta Arenas, Chile Posts: 62 Rep Power: 9 ghorrocks; sorry for that stupid question about the mass flow rate boundary! i really dont know what i was thinking. 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 , the first think that imgona do finishing this work, its sleep long time! best regards

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Saturn CFX 45 February 8, 2016 05:42 Pankaj CFX 9 November 23, 2009 05:05 saii CFX 2 September 18, 2009 08:07 Mark CFX 6 November 15, 2004 16:55 Tudor Miron CFX 15 April 2, 2004 06:18

All times are GMT -4. The time now is 23:17.