CFD Online Logo CFD Online URL
Home > Forums > Software User Forums > ANSYS > CFX

Acoustic boundary condition with pressure perturbation at inlet

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

LinkBack Thread Tools Search this Thread Display Modes
Old   June 29, 2018, 11:06
Default Acoustic boundary condition with pressure perturbation at inlet
Join Date: Nov 2017
Posts: 37
Rep Power: 8
hand90 is on a distinguished road
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.
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?
hand90 is offline   Reply With Quote

Old   June 30, 2018, 05:56
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,703
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
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.
ghorrocks is offline   Reply With Quote

Old   August 10, 2018, 07:36
Join Date: Nov 2017
Posts: 37
Rep Power: 8
hand90 is on a distinguished road
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.
hand90 is offline   Reply With Quote


acoustic reflectivity, cfx, opening boundary

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

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 Off
Trackbacks are Off
Pingbacks are On
Refbacks are On

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 06:08
Multiphase flow - incorrect velocity on inlet Mike_Tom CFX 6 September 29, 2016 01:27
Question about heat transfer coefficient setting for CFX Anna Tian CFX 1 June 16, 2013 06:28
Low Mixing time Problem Mavier CFX 5 April 29, 2013 00:00
what the result is negatif pressure at inlet chong chee nan FLUENT 0 December 29, 2001 05:13

All times are GMT -4. The time now is 19:35.