Acoustic boundary condition with pressure perturbation at inlet

hand90 · June 29, 2018, 12:06

Hello everyone

In my 2D simulation I am interested how pressure waves convect through a duct (later on through a 3D turbine stage). For this I need non-reflective boundary conditions. As mentioned in other posts this is a Beta setting in CFX and requires an Opening as boundary condition at the inlet and outlet. As I don't want any reflection I have set the Reflection Factor at the inlet and outlet to 0.

About the simulation:

Inlet: Opening Pressure and Direction, the pressure is a set to a mean pressure with a 300Hz perturbation of 1.9kPa. Relative pressure =140[kPa]+1.9[kPa]*sin(2*pi*300[Hz]*t)
Outlet: Static Pressure and Direction
Upper and lower domain boundaries are set as wall while the side walls are set as symmetry

The simulation is initiated with steady state simulation which converged very quick (no pressure perturbation modeled).
When moving to the transient simulation I get the following error:
ERROR #004100018 has occurred in subroutine FINMES.
Message:
Fatal overflow in linear solver.

However, I have ran the exact same simulation with a pressure perturbation without the acoustic boundary condition and an inlet and outlet instead of an opening and that worked with no problem.

My question is, what are the correct boundary conditions for an acoustic simulation with no reflection at the inlet and outlet, and where did I go wrong in my setup?

ghorrocks · June 30, 2018, 06:56

That is the problem with beta features. They are not always stable or reliable. That is why it is not a released feature. So try the normal things for numerical instability: smaller time step, double precision numerics, improved mesh quality and better initial conditions.

There are other ways you can do non-reflecting boundary conditions. One method is by grossly coarsening the grid at the boundary, probably using a GGI boundary. When the pressure wave hits the coarse grid it will be attenuated due to numerical dissipation. Another method is to have really long inlet and outlet duct such that the reflections don't get back to the region of interest within the simulation time. Finally you can put physical features which attenuate the waves - like a muffler - on the duct.

hand90 · August 10, 2018, 08:36

Thank you very much for your help!

As you mentioned the acoustic feature within CFX are very unstable and I will have to see if I will be successful with them at a later stage. However in the mean time I was able to get a converged solution by decreasing the time step (1e-5s). I have also tried using a long buffer zone with a coarse mesh. This definitely is an option, however it also introduces a lot of numerical noise.

June 29, 2018, 12:06	Acoustic boundary condition with pressure perturbation at inlet	#1
hand90 Member Thomas Join Date: Nov 2017 Posts: 37 Rep Power: 9	Hello everyone In my 2D simulation I am interested how pressure waves convect through a duct (later on through a 3D turbine stage). For this I need non-reflective boundary conditions. As mentioned in other posts this is a Beta setting in CFX and requires an Opening as boundary condition at the inlet and outlet. As I don't want any reflection I have set the Reflection Factor at the inlet and outlet to 0. About the simulation: Inlet: Opening Pressure and Direction, the pressure is a set to a mean pressure with a 300Hz perturbation of 1.9kPa. Relative pressure =140[kPa]+1.9[kPa]sin(2pi300[Hz]t) Outlet: Static Pressure and Direction Upper and lower domain boundaries are set as wall while the side walls are set as symmetry The simulation is initiated with steady state simulation which converged very quick (no pressure perturbation modeled). When moving to the transient simulation I get the following error: ERROR #004100018 has occurred in subroutine FINMES. Message: Fatal overflow in linear solver. However, I have ran the exact same simulation with a pressure perturbation without the acoustic boundary condition and an inlet and outlet instead of an opening and that worked with no problem. My question is, what are the correct boundary conditions for an acoustic simulation with no reflection at the inlet and outlet, and where did I go wrong in my setup?

June 30, 2018, 06:56		#2
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,854 Rep Power: 144	That is the problem with beta features. They are not always stable or reliable. That is why it is not a released feature. So try the normal things for numerical instability: smaller time step, double precision numerics, improved mesh quality and better initial conditions. There are other ways you can do non-reflecting boundary conditions. One method is by grossly coarsening the grid at the boundary, probably using a GGI boundary. When the pressure wave hits the coarse grid it will be attenuated due to numerical dissipation. Another method is to have really long inlet and outlet duct such that the reflections don't get back to the region of interest within the simulation time. Finally you can put physical features which attenuate the waves - like a muffler - on the duct. __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Pressure Inlet Boundary Condition for gas-solid fluidized bed	m.uzair	Fluent Multiphase	0	January 18, 2018 07:08
Multiphase flow - incorrect velocity on inlet	Mike_Tom	CFX	6	September 29, 2016 02:27
Question about heat transfer coefficient setting for CFX	Anna Tian	CFX	1	June 16, 2013 07:28
Low Mixing time Problem	Mavier	CFX	5	April 29, 2013 01:00
what the result is negatif pressure at inlet	chong chee nan	FLUENT	0	December 29, 2001 06:13

August 10, 2018, 08:36		#3
hand90 Member Thomas Join Date: Nov 2017 Posts: 37 Rep Power: 9	Thank you very much for your help! As you mentioned the acoustic feature within CFX are very unstable and I will have to see if I will be successful with them at a later stage. However in the mean time I was able to get a converged solution by decreasing the time step (1e-5s). I have also tried using a long buffer zone with a coarse mesh. This definitely is an option, however it also introduces a lot of numerical noise.