CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   Fan type BC in OF15 (http://www.cfd-online.com/Forums/openfoam-solving/57907-fan-type-bc-of15.html)

hsieh July 15, 2008 21:13

Hi, I notice fan type BC in
 
Hi,

I notice fan type BC in OF-1.5. Had anyone tried it yet? Does anyone knows how to use it?

pei

eugene July 16, 2008 07:00

The fan boundary is an interna
 
The fan boundary is an internal coupled patch (cyclic) with a scalar jump for pressure. Basically a jump boundary.

hsieh July 16, 2008 08:22

Hi, Eugene, Thanks for the
 
Hi, Eugene,

Thanks for the answer. Is there any example on how to use it?

Pei

hsieh July 17, 2008 08:27

Hi, Eugene, I am considerin
 
Hi, Eugene,

I am considering using the fan type BC to model a fan inside fluid domain. A fan has an intake and an outlet (back into the fluid domain). If the pressure at far field is 0, then, the intake side of the fan might be negative, then, there is a pressure jump to the outlet (this pressure may be positive).

Can the fan type BC handle something like this? That is, specify low pressure on the fan intake side, and then, a pressure jump for the whole fan?

Pei

eugene July 17, 2008 08:56

I didn't write this BC, so alt
 
I didn't write this BC, so although I have based some development off it, don't take my word as writ. Basically this boundary effects a pressure jump. Cross in one direction and the pressure increases, cross in the other and it decreases.

Unfortunately I don't have an example of its usage. I can say that it works on top of a cyclic type boundary though. This means all the other flow fields will have a cyclic (or cyclic derived) boundary at the location of the fan.

So to answer your questions yes and yes.

hsieh July 17, 2008 22:06

Thanks again, Eugene! Pei
 
Thanks again, Eugene!

Pei

podallaire July 27, 2008 12:17

Good morning, I understand
 
Good morning,

I understand that the new fan BC adds a pressure jump on an internal boundary (surface). For this BC, how is defined the velocity ? Is is possible to use the fan bc and specify a velocity profile at the fan outlet (using funkysetfield) ?

I already have a case where a thin cylinder was grooved and removed from the mesh. I applied some bcs on the two circular surfaces in order to simulate the fan inlet/outlet behavior. My fan is in a room. A pressureInlet bc was specified for the room inlet and the pressureInletOutlet bc was used for the room outlet. I'd like to try this new fan bc but did not find any specific example case using it.

Best regards,

PO

eugene July 28, 2008 05:35

You will not be able to specif
 
You will not be able to specify the velocity at the jump boundary without some user coding. At the moment there are only 2 boundaries that can coincide with an internal boundary: cyclic and jumpCyclic. To do what you want, you will have to derive a new BC type that can sit on top of a cyclic patch, but behave like a fixed value.

Unfortunately, this might be quite tricky.

saasebo February 24, 2009 07:00

Hello http://www.cfd-online.co
 
Hello http://www.cfd-online.com/OpenFOAM_D...part/happy.gif

I do not find any examples of how to assign this fan boundary condition. Are there anyone who have done this before?

Best regards, Steinar

vinz March 18, 2009 03:57

Hi everyone,

Thanks to Eugene I understood that the internal faces are treated with a cyclic boundary condition in OpenFOAM.
I also would like to use the fan boundary condition to impose a pressure jump through an internal surface. My problem is that I don't know how to set up the boundary condition files.
For the boundary of interest named disk, i have the following:
in p file:
disk
{
type cylic;
value uniform -1000;
}
in U file:
disk
{
type cyclic;
}
in boundary file:
disk
{
type cyclic;
nFaces 640;
startFace 53760;
}
If I impose the conditions above, there is no pressure jump happening during the computation with simpleFoam.
Could one of you tell me how to set up those boundary conditions to get a pressure jump?
Thanks in advance.

Vincent

saasebo April 15, 2009 11:55

Dear Foamers

The fan boundary condition is working on a cyclic patch (named ad here) defined in constant/polyMesh/boundary as

ad
{
type cyclic;
}

and then in the pressure file 0/p:

ad
{
type fan;
patchType cyclic;
f List<scalar> 2(10.0 -1.0);
value uniform 0;
}

The f above is a list of polynomial coefficients in the pressure jump definition

delta p = f_1 + f_2 * v + f_3 * v^2 + ...

Above only f_1 and f_2 is assigned, respectively 10.0 and -1.0.

In 0/U and so on, the ad patch is defined as cyclic.

My problem is now:
Is it possible to assign nonuniform coefficients f along the patch, e.g. if I want to assign a nonuniform pressure jump independent of velocity (using only f_1)?

Best Regards
Steinar

roth April 17, 2009 14:08

Example case
 
1 Attachment(s)
Thanks Steinar. Here's an example for flow down a duct driven by a fan in the middle.
Mike

powen July 17, 2009 16:52

What is the "featureCos" in the boundary file? It is set to 0.9

What's the definition?

maddalena April 30, 2010 03:03

Quote:

Originally Posted by saasebo (Post 213028)
... and then in the pressure file 0/p:

ad
{
type fan;
patchType cyclic;
f List<scalar> 2(10.0 -1.0);
value uniform 0;
}

The f above is a list of polynomial coefficients in the pressure jump definition

delta p = f_1 + f_2 * v + f_3 * v^2 + ...

Above only f_1 and f_2 is assigned, respectively 10.0 and -1.0.

In 0/U and so on, the ad patch is defined as cyclic.

Hello Steinar,
could you explain me how I set the sign of pressure difference? How can I understand if I have to set the delta p is positive or negative before running the case itself? Thank you!

saasebo April 30, 2010 07:06

Hello,

For a fan, you probably want a positive pressure jump when moving through the fan in the velocity direction (from suction side to pressure side). But if it is the order of patches in the cyclic, or the coordinate system that tells if f_1 should be positive also, I don't remember. You will see it quite quick if the pressure jump has wrong direction.

BR, Steinar

kh_mohsen_m2 June 16, 2010 05:05

A Reqest
 
Hello,
Are you have any information about Intake-fan Boundry condition? I have a project about Intake fan, that have a problem, can you help me ? in the other hand i need 2 example about intake-fan.
Thank u for reply.:(:)

maddalena September 14, 2010 03:59

...thinking to what Eugene posted above...
Quote:

Originally Posted by eugene (Post 193325)
Basically this boundary effects a pressure jump. Cross in one direction and the pressure increases, cross in the other and it decreases.

1) Does this mean that the flow can go in both directions at the same time? Since the fan bc is based on a cyclic boundary, I guess this may be possible.
2) Does this mean that the fan can be used as a sort of local losses to simulate the pressure drop on a system that does not need to be modeled?

mad

olivierG September 14, 2010 08:27

hello maddalena,

for 1), i would say yes, but i am a new user here ...
for 2), yes, you can use fan as a porous jump to model flow through a grid ... but maybe not in 1.6 or 1.7 see
http://www.cfd-online.com/Forums/openfoam/79757-fan-patch-acting-porous-jump.html
I am actually looking at how to get an internal boundary from gambit mesh to get it in polymesh/boundary, in order to use cyclic BC, and i will try this "porous jump"

Olivier

maddalena September 14, 2010 08:32

Hello Olivier,
I noticed that post but none has replied yet. however, I always set the deltaP value positive or negative according to my mesh, and never had any problem in OF 1.6...
Let me know how your test will go.
Cheers,

mad

maddalena September 15, 2010 06:14

3 Attachment(s)
Hi everyone,
following the discussion of yesterday with Olivier and on the basis of some problems I have met, I played a bit with the tutorial fan case posted above. I studied the laminar case, to keep things simple. the solution is as in picture orig.png.
First, I tried to invert the flow direction, i.e. instead of going from left to right, I wanted it to go from right to left. Thus, I exchanged the boundary conditions and changed sign (from positive to negative) to fan f coefficient. Results are shown in picture bc.png: the fan misbehaves.
Another method of reversing the flow direction is to exchange boundary conditions and invert the order of the cyclic definition, using a positive f coefficient. Therefore, on a second set, I changed the master and slave face order on blockMeshDict: from:
Code:

    cyclic fan
    (
        ( 1 2 6 5 ) //master
        ( 8 12 15 11 ) //slave
    )

to
Code:

    cyclic fan
    (
        ( 8 12 15 11 ) //master
        ( 1 2 6 5 )//slave
    )

Results are shown in bcOrd.png: the flow direction is reversed and results are as expected.

Conclusion: on OF 1.6 and 1.7, the f coefficient must be positive, the flow direction is set by the master and slave face of the cyclic condition.

Open point: can the fan BC be used to simulate local losses? What happens if the flow approaching the fan has a direction opposite to the supposed positive direction for the fan?

mad


All times are GMT -4. The time now is 05:33.