[mfinke]

Dear community members,

i working on a "displacement pump" model. The Fluid is defined as 1 phase compressibel flow (roh = f(p)) and a turbulence model is used.

Inlet and Outlet is defined as opening with pressure boundary condition with the nonreflective beta feature activated.

There are several GGIs defined to connect different parts of the pump (e.g. pistons with control journal).

Its a transient simulation with moving mesh regions.

I´m using initial condtions from earlier simulation with reflective B.C. but large time step where the pressure wave propagation has no influence on flow behaviour.

Problem:
due to the constant pressure boundary conditions i have numeric pressure wave reflections at the Inlet and Outlet and later on propagation of this waves.

Therefore I´m trying to use the nonreflective boundary condtion option in CFX-Pre but in the first Iteration i get the following error message:

"ERROR #001100279 has occurred in subroutine ErrAction.
Message:Signal caught: Segmentation violation"

"ERROR #001100279 has occurred in subroutine ErrAction.
Message: Stopped in routine SIG_HANDLER:"

any idea ?
Is there some limitation of this beta feature ?
I only know that nonreflective B.C. don´t works together with multiphase flows.

best regards and thank you in advance

Matthias

[mfinke]

Dear members,
i´m still working on the problem. Meanwhile we find out that mesh motion has no influence on the error message.
Now i´m trying to figure out if grid Interfaces could be a source for the error. You are welcome to share your experience with me.

best regards

Matthias

[ghorrocks]

That's probably why it is still in beta.

Just a wild idea, but try replacing the non-reflective boundary with a really coarse mesh just at the boundary. Connect it to the main domain with a GGI and put a normal pressure boundary at the exit. Very coarse meshes have high dissipation and you may be able to get a non-reflective (or at least not very reflective) boundary out of that.

[joey2007]

Glenn´s approach is quite practical.

Do you use a turbulence resolving approach (LES, SAS, DES)? Then a coarse mesh may destroy also vortices flow upwards. Do not know if that is accurate. Unfortunately I do not have a better solution . If it is a scientific work, you may check:

A. Widenhorn, B. Noll, M. Aigner
Impedance boundary conditions for the numerical simulation of gas turbine combustion systems
ASME GT2008-50445, 2008

[mfinke]

Dear members,

thank you for the suggestions made for my problem.

I have already tried to extrude the inlet and outlet (l=10m) of the pump. I used a bunching law for the extruded meshes (10 elements, 1st element hight 0,003m).

There reflection of the pressure wave were still there. I think i need to adapt the mesh density and pipe lenght and bondary condition type (see ghorrocks) to smooth/eliminate the pressure waves reflection. (a=1220 [m/s]@ high pressure pipe; a=200 [m/s] low pessure pipe; tsimulation = 2 x 0.033 [s])

Joey2007: thank you for the literature source. Hope your financial situation is ok ;-)

best regards

MAtthias

[joey2007]

@Matthias: It is okay. I just wanted to remember some folks here, that you never have to look into the mouth of a gifted horse. Guess you may understand what I mean, if not it is not so important ....

[alinik]

Hey mfinke
were you able to resolve that error message?

Thanks

[mfinke]

Hey alinik,

yes i was, as i remember there were two possible reasons for the problem:
=> negative slope of density(p)-function ( while increasing pressure, density should increase also)
=> type of partition in distributed parallel runs

hope this helps

best regards

[alinik]

Originally Posted by mfinke

Hey alinik,

yes i was, as i remember there were two possible reasons for the problem:
=> negative slope of density(p)-function ( while increasing pressure, density should increase also)
=> type of partition in distributed parallel runs

hope this helps

best regards

Thanks mfinke for your quick reply,

Since I am running it serial mode so it could not be a result of the second reason. Also I am modeling the flow around an airfoil at low Mach number so the flow could be assumed as incompressible(constrant density).
It has to be because of something else.
The fact is I am trying to impose the inlet BC using a fortran code. I am not sure if this is related to that fact. I receive absolutely no error while compiling the code and introducing the routine, function and inlet CEL. So it also seems that the fortran code and everything is fine.
I am desperatley looking for some solution to this error.

Any kind of information that might help is greatly appreciated.

Thanks

Ali,