|
[Sponsors] |
![]() |
![]() |
#1 |
Senior Member
Sakun
Join Date: Nov 2019
Location: United Kingdom
Posts: 107
Rep Power: 6 ![]() |
Hello everyone,
I simulating 0.7 mach number simulation for a single compressor blade using rhoPimpleFoam. Simulation is pressure based so i just have to set up INLET flow direction and OUTLET flow direction. I have already set up INLET flow (45.83 degrees)direction using "pressureDirectedInletVelocity" but i don't know any boundary condition to set up OUTLET flow direction which is 6.22. Can i get some suggestion for this issue ![]() Thank you very much for your time, Code:
/*--------------------------------*- C++ -*----------------------------------* \ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: v2112 | | \\ / A nd | Website: www.openfoam.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class volVectorField; object U; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 1 -1 0 0 0 0]; internalField uniform (0 0 0); boundaryField { INLET { type pressureDirectedInletVelocity; inletDirection uniform (0.631623456 -0.775275312 0); //geometric inlet angle is 50.83 value uniform (0 0 0); } OUTLET { type pressureInletOutletVelocity; inletValue uniform (0 0 0); value uniform (0 0 0); } CASCADE { type noSlip; } "(TOP|BOTTOM)" { type cyclicAMI; } frontAndBackPlanes { type empty; } } // ************************************************************************* // |
|
![]() |
![]() |
![]() |
![]() |
#2 | |
Member
Alejandro Valeije
Join Date: Nov 2014
Location: Spain
Posts: 52
Rep Power: 11 ![]() |
Hi,
Although I haven't played with it, maybe you can try with pressureDirectedInletOutletVelocity, setting the outflow direction properly. I'll let you the link with the definition: https://www.openfoam.com/documentati...8H_source.html Let me know if it works. Regards, Quote:
|
||
![]() |
![]() |
![]() |
![]() |
#3 | |
Senior Member
Sakun
Join Date: Nov 2019
Location: United Kingdom
Posts: 107
Rep Power: 6 ![]() |
Quote:
Hi , Thank you very much for the reply. I had this boundary condition in my mind but since it said "inletDirection" again, i thought it only works with INLETs ![]() Code:
{ type pressureDirectedInletOutletVelocity; phi phi; rho rho; inletDirection uniform (1 0 0); value uniform 0; } ![]() Code:
{ type pressureDirectedInletOutletVelocity; phi phi; rho rho; inletDirection uniform (0.9941 0.1083 0);//[cos6.22 sin6.22 0] value uniform 0; } |
||
![]() |
![]() |
![]() |
![]() |
#4 | |
Member
Alejandro Valeije
Join Date: Nov 2014
Location: Spain
Posts: 52
Rep Power: 11 ![]() |
Hi Sakun,
As far as I understand, I would proceed as you have written. In any case, if you have any concern whether this is going to work and your case is too big, you can create a simple straight channel and try there the boundary conditions. The case only needs to have inlet, outlet and walls and it will run almost inmediately. Best regards, Quote:
|
||
![]() |
![]() |
![]() |
![]() |
#5 | |||
Senior Member
Yann
Join Date: Apr 2012
Location: France
Posts: 1,169
Rep Power: 27 ![]() |
Hello,
Quote:
Quote:
Quote:
Regards, Yann |
||||
![]() |
![]() |
![]() |
![]() |
#6 | |
Senior Member
Sakun
Join Date: Nov 2019
Location: United Kingdom
Posts: 107
Rep Power: 6 ![]() |
Quote:
Hi Alejandro, I can't really make it straight at the OUTLET becasue this is turbomachinery simulation and i had to follow the exact domain shape that my reference paper has ![]() Best regards, Sakun |
||
![]() |
![]() |
![]() |
![]() |
#7 | |
Senior Member
Sakun
Join Date: Nov 2019
Location: United Kingdom
Posts: 107
Rep Power: 6 ![]() |
Quote:
Hi Yann, Thank you very much for your kind response my isseue, i higly appriciate that ![]() In that case i can either use "pressureDirectedInletOutletVelocity" or "pressureDirectedInletVelocity" for the INLET and use "zeroGradient" for the OUTLET ? Best regards, Sakun |
||
![]() |
![]() |
![]() |
![]() |
#8 | |
Senior Member
Yann
Join Date: Apr 2012
Location: France
Posts: 1,169
Rep Power: 27 ![]() |
Quote:
Yes it sounds good. I guess you won't have backflow at the inlet, so pressureDirectedInletVelocity should do the job. Cheers, Yann |
||
![]() |
![]() |
![]() |
![]() |
#9 | |
Senior Member
Sakun
Join Date: Nov 2019
Location: United Kingdom
Posts: 107
Rep Power: 6 ![]() |
Quote:
Hi Yann, Thank you very much for the suggestion, i will work on you suggestion ![]() Since i have periodic boundary conditions for TOP and BOTTOM (attached picture) flow is extremely unsteady (go beyond 300 m/s) and it affects the stablity of the simulation too much ![]() So hopefully i guess zeroGradient in the OUTLET boundary condition would do the work. Best regards, Sakun |
||
![]() |
![]() |
![]() |
Tags |
flow direction, periodic boundaries, turbo machinery, unsteady compressible |
|
|
![]() |
||||
Thread | Thread Starter | Forum | Replies | Last Post |
Simple Box - Gravity with Pressure Outlet - Unrealistic Reverse Flow | pyccknn | FLUENT | 2 | December 1, 2021 17:31 |
setting OUTLET flow rate equal to INLET flow rate | spitchers | OpenFOAM Programming & Development | 0 | March 22, 2018 06:33 |
Compressible Flow Pressure Outlet Back Flow | okstatecheme | OpenFOAM Running, Solving & CFD | 1 | March 21, 2018 08:11 |
ATTENTION! Reliability problems in CFX 5.7 | Joseph | CFX | 14 | April 20, 2010 15:45 |
Warning 097- | AB | Siemens | 6 | November 15, 2004 04:41 |