CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   Main CFD Forum (http://www.cfd-online.com/Forums/main/)
-   -   Opening Boundary Condition (http://www.cfd-online.com/Forums/main/114802-opening-boundary-condition.html)

 andreachan March 18, 2013 05:53

Opening Boundary Condition

Hello,

I want to simulate a flow domain having such a boundary, where the pressure value is known, and the fluid can flow into or out of the domain at this boundary. It means this boundary can be an inlet or outlet boundary conditions with fixed pressure value.

I am wondering how to treat the pressure and velocity on this boundary, since the flow direction can be both in and out. Is it correct that I treat the boundary as normal inlet pressure static BC when the fluid flows in and as normal outlet pressure static BC when the fluid flows out?

I have found such a boundary condition in the software CFX, which is called Opening Boundary Condition.

I am wondering the principle and mathematical background of this boundary condition. However, I could not find any details in the CFX manual.

Thanks.

 FMDenaro March 18, 2013 09:00

I don't understand your flow problem...what about your computational domain and the forces driving the main flow?

 andreachan March 18, 2013 09:30

There is a movable part in the domain, which makes the volume of the whole domain changeable. When the volume decreases, the fluid flows out through this 'opening boundary'. When the volume increases, the fluid flows in through this 'opening boundary'.

Quote:
 Originally Posted by FMDenaro (Post 414672) I don't understand your flow problem...what about your computational domain and the forces driving the main flow?

 FMDenaro March 18, 2013 11:00

Quote:
 Originally Posted by andreachan (Post 414677) There is a movable part in the domain, which makes the volume of the whole domain changeable. When the volume decreases, the fluid flows out through this 'opening boundary'. When the volume increases, the fluid flows in through this 'opening boundary'.
if the flow is modelled as incompressible, you can set also some bc. on the velocity instead of pressure, for example setting a vanishing second derivative. If the flow is fully compressible, you need some more complex non-reflecting bc.s.

 andreachan March 18, 2013 13:54

Quote:
 Originally Posted by FMDenaro (Post 414705) if the flow is modelled as incompressible, you can set also some bc. on the velocity instead of pressure, for example setting a vanishing second derivative. If the flow is fully compressible, you need some more complex non-reflecting bc.s.
I am simulating an incompressible fluid. But I wondering why we can set a vanishing second derivative of the velocity as a boundary condition. What is the physical meaning of it?

 FMDenaro March 18, 2013 14:01

Quote:
 Originally Posted by andreachan (Post 414762) Thanks Filippo for your advise. I am simulating an incompressible fluid. But I wondering why we can set a vanishing second derivative of the velocity as a boundary condition. What is the physical meaning of it?
you have to distinguish between the correct mathematical BC and its consequent physical meaning.
For incompressible flows you can prescribe either velocity or pressure to have the problem well posed. What the physics says you about the inlet/outle? I don't think you know the velocity profile or the pressure gradient in time ... therefore some "free condition" on the velocity is better to let the flow to go in and out. You cna also prescribe some fixed pressure value if you have two large tank at the end...
What is really required is that you enforce correctly the divergence-free constraint

 Jonas Holdeman March 19, 2013 00:05

Open boundary condition

2 Attachment(s)
Quote:
 Originally Posted by andreachan (Post 414632) Hello, I have found such a boundary condition in the software CFX, which is called Opening Boundary Condition. I am wondering the principle and mathematical background of this boundary condition. However, I could not find any details in the CFX manual. Could anyone tell me some papers or books about this kind of boundary condition? Thanks.
Attached is an FEM example using "open boundary conditions" or "do-nothing" b.c. This involves a benchmark problem, the simplified backward facing step, where the inlet throat is omitted with the assumption that the entrance flow has a parabolic profile. I have used Re=800. There are primary and secondary recirculation bubbles. The first mesh length (7 x channel height) is chosen so that the exit passes through the second bubble. The fluid is flowing both in and out and clearly it is not the case that the derivative is zero on exit boundary. In the second image the mesh was truncated through the first recirculation bubble with mesh length 3 x channel height and is seen to be consistent with the longer mesh. There is, of course, a truncation boundary layer, but it is very small as seen from the figures.

 andy_ March 19, 2013 07:11

Quote:
 Originally Posted by andreachan (Post 414677) There is a movable part in the domain, which makes the volume of the whole domain changeable. When the volume decreases, the fluid flows out through this 'opening boundary'. When the volume increases, the fluid flows in through this 'opening boundary'.
Setting physically reasonable boundary conditions for 'open' inflows can be tricky and require a bit of experimentation. Simply fixing the static pressure can be OK if the flow is gently flapping about but if there is a significant dynamic pressure in the backflow then some form of total pressure condition is likely to be more physically reasonable.

I am not familiar with the current set of CFX boundary conditions and so can offer little help here.

 andreachan March 19, 2013 07:14

Quote:
 Originally Posted by Jonas Holdeman (Post 414847) Attached is an FEM example using "open boundary conditions" or "do-nothing" b.c. This involves a benchmark problem, the simplified backward facing step, where the inlet throat is omitted with the assumption that the entrance flow has a parabolic profile. I have used Re=800. There are primary and secondary recirculation bubbles. The first mesh length (7 x channel height) is chosen so that the exit passes through the second bubble. The fluid is flowing both in and out and clearly it is not the case that the derivative is zero on exit boundary. In the second image the mesh was truncated through the first recirculation bubble with mesh length 3 x channel height and is seen to be consistent with the longer mesh. There is, of course, a truncation boundary layer, but it is very small as seen from the figures.
Thanks Jonas for your detailed explanation with figures.

Do you also know the mathematical description of such boundary condition?

 andreachan March 19, 2013 07:20

Quote:
 Originally Posted by FMDenaro (Post 414766) you have to distinguish between the correct mathematical BC and its consequent physical meaning. For incompressible flows you can prescribe either velocity or pressure to have the problem well posed. What the physics says you about the inlet/outle? I don't think you know the velocity profile or the pressure gradient in time ... therefore some "free condition" on the velocity is better to let the flow to go in and out. You cna also prescribe some fixed pressure value if you have two large tank at the end... What is really required is that you enforce correctly the divergence-free constraint
If I set a fixed value of pressure on this boundary. Should I do something on the velocity components from the numerical point of view? E.g. setting a zero gradient of the velocity on this boundary.

 Jonas Holdeman March 19, 2013 11:08

open boundary condition

1 Attachment(s)
I thought about this a little more and did a Google search on open boundary conditions. Most of the hits seemed to involve atmospheric or oceanic flows and radiation, and the methods seem mostly heuristic. My examples involve a specific method, but perhaps there are general considerations.

Quote:
 Originally Posted by andreachan (Post 414942) Do you also know the mathematical description of such boundary condition?
In my example, mass is strongly conserved. This is done (in 2D) by using modified Hermite elements for the stream function, where the derivative terms are the velocity (it could be called a stream function - velocity method). The velocity elements are the curl of the stream function element and hence are strongly divergence-free. I think it might work when truncating the mesh through a recirculation bubble because any fluid outflow carried out through an open face, say by its momentum, must be replaced by an equal inflow. Perhaps the condition needed is that mass conservation must be strong and independent of what is happening at the outflow.

In my case, the equations for the nodes on the exit face are only partially assembled because here are no elements outside. This may be called a "do nothing" boundary condition. I am not sure why it works, but it does. Any mathematicians out there?

This open condition has further utility. Consider flow over a cylinder. One usually uses a mesh wide enough that the effects of truncation of the space might be neglected. Usually one has to compromise between computational work and accuracy. But suppose you leave the top and bottom of the mesh open as well. Then the fluid could expand outside the mesh near the cylinder, and then re-entering downstream, reducing the influence of truncation without additional work. This is shown for Re=50 in the figure, where the top, bottom and right end are open, but net flow through the top and bottom constrained to be zero.

 leflix March 19, 2013 17:46

Quote:
 Originally Posted by andreachan (Post 414944) If I set a fixed value of pressure on this boundary. Should I do something on the velocity components from the numerical point of view? E.g. setting a zero gradient of the velocity on this boundary.
Yes zero gradient is an option, from a physical point of view it indicates that the velocity is the same on each side of the boundary. A better one is, as Filippo stated it, second derivative of the velocity =0. In this case you specify that you want to keep the same gradient of the velocity on each side of the boundary. This BC is less constraining for the solution.

 All times are GMT -4. The time now is 04:41.