[robingilbert]

Hi,

I want to force a fluid at a constant flow rate through a small area inside the fluid domain. I know about the cyclic boundary condition but i do not know how to set it up so that it will give a constant flow rate. I looked into channelFoam and i know how to modify the simpleFoam solver so that it can fix the flowrate. but i just cant figure out how to make it so that the forcing is only through a small area inside the fluid domain.
I considered adding a forcing term to the UEqn which is something like:

(v/A-U)*alpha

where v is volume flow rate
A-area of the surface
U- current velocity at the surface
alpha- a term which has dimensions 1/time which can drive down the solution to required flow rate.
is this approach right?

Please give me some pointers.

[eugene]

The only way to do what you want, is literally to have a fixed mass flow outlet adjacent to a fixed flow inlet that maps the velocity from the adjacent outlet (and vice-versa for pressure). You can do this by starting from the low level coupled patches (cyclics), but it isn't trivial unless you know what you are doing and the resulting system probably wont be very stable. Unfortunately I don't think there is an easy solution for this particular aspect of the problem.

A different approach is to put in something like an actuator disc from 1.7 wind solver and adjust the driving force such that the flow rate approximates your target value.

[robingilbert]

Thank you Eugene,

I will try the actuator disk and see if that works.
So according to ur first suggestion, do i need to make a hollow volume without any meshes and has an inlet (into the fluid domain) and an outlet (into the hollow volume) and map the velocity from inlet to the outlet?

[eugene]

Originally Posted by robingilbert

Thank you Eugene,

I will try the actuator disk and see if that works.
So according to ur first suggestion, do i need to make a hollow volume without any meshes and has an inlet (into the fluid domain) and an outlet (into the hollow volume) and map the velocity from inlet to the outlet?

No, no - no holes required. You take your basic cyclic boundary (which can act just like an internal boundary) and start chopping and changing. For U you want one side of the cyclic patch pair to be a scaled "zero gradient" outlet such that the total flux matches your specification. The other side is an inlet that simply gets its value from the outlet side, just like a normal cyclic. For pressure, you want the reverse, the inlet side is zero gradient and this value is mapped to the outlet side and treated as fixed. The switching is done based on flux direction. I did something like this at my previous job and remember that it was a bit tricky. Unfortunately I don't have the code any more, but it is certainly possible.

[robingilbert]

Thanks once again Eugene.
one more question. forgive me if its a stupid question, can I add a source term in the momentum eqn so that it will force the fluid at a particular flow rate?

[eugene]

Of course. I pointed you toward the actuator disk because this is exactly the framework you need to implement the source term you need. An example usage can be found here: OpenFOAM-1.7.x/tutorials/incompressible/simpleWindFoam and the source code for the actuator disk and base class can be found here: OpenFOAM-1.7.x/src/finiteVolume/cfdTools/general/fieldSources/basicSource

[robingilbert]

Thank you soooooooooo much Eugene. I will try that out!! thank you once again.

[maddalena]

Hi Robin,
I probably need something similar for this kind of problem: http://www.cfd-online.com/Forums/ope...flow-rate.html. Eugene suggested me to modify the actuator disk model as well. Have you made any progress on the subject? Shall we collaborate?
Regards

mad