CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FloEFD, FloWorks & FloTHERM (http://www.cfd-online.com/Forums/floefd-floworks-flotherm/)
-   -   Setting Flow/Pressure Boundaries in Floworks (http://www.cfd-online.com/Forums/floefd-floworks-flotherm/66487-setting-flow-pressure-boundaries-floworks.html)

Eran July 16, 2009 18:04

Setting Flow/Pressure Boundaries in Floworks
 
Dear All,

I am working on simulating air flow in an existing model. The model has two air inlets and one outlet. The inlets are on opposing sides of the symmetrical model.

Currently I only know that 80 mL/min of air is coming from each of the inlets and of course 160 mL/min from the outlet. The air is pulled by creating a small vacuum on the outlet while the inlets are exposed to the atmospheric pressure.

Since I am new to Floworks I am encountering problems in setting the boundaries. I tried to set only flow boundaries on the inlets and outlet, however, I received an error message that the model has to have pressure boundaries to work. Since I donít know the pressure differential between the inlet and outlet (I only know the air flow), this is a problem. I tried to set some arbitrary pressure in the inlet (you cannot set a negative pressure in the outlet), but I get some very high flows which do not make any sense.

My question: Is it possible to set only flow boundaries without pressure boundaries

Boris_M July 20, 2009 06:01

BCs, how to...
 
Hi Eran,

you'll need either pressure BCs for inlet and outlet or pressure and flow BCs. This is due to two basic equations that have to be defined with that. it's the mass continuity and bernulli.

Mass continuity: what goes in has to come out again

v*A*rho=m

so either you define the velocity (v), the volume flow rate (v*A) where A is the cross section surfacearea or the mass flow (with rho as density).

Bernulli: basically an energy balance

p_static + p_dynamic + p_potential = p_total

p_dynamic = 1/2 * rho * v^2
p_potential = rho * g * h

rho is the desnity again, v the velocity, g is the acceleration due to gravity and h is the hight.

As you can see if you define two pressures on inlet and outlet you would automatically define a difference between the pressures that would be a loss due to the systems geometry and therfore the velocity would be iterated in the equation automatically but if you define mass flow on in and outlet this would be already defined by the mass balance but what would be the pressure?
Can you see that you will at least need one pressure?

Of corse there are no negative pressures. Pressures are always absolute (which means above absolute vacuum = 0 Pa). Usually valve and pump manufacturers use pressures above or below environment pressure (101325 Pa). So if they are talking about 50 Pa negative pressure you'll have to say it is 50 Pa below environment pressure so 101325 Pa - 50 Pa = 101275 Pa.

Oh, and please don't mix the definition of the physical environment pressure with the one in FloEFD. The one in FloEFD just determines that it is toal pressure if the flow is entereing the system on this BC or if it is static pressure if the flow leaves the system.

If you don't have any data about the pressure check the way you would test your model on a test stand. You usually have somehow either a pump that generates a pressure or it generates a constant volume flow or something like that. You can also use the fan curve if you have the pumps curve.

I hope this helps you. :)

Eran July 22, 2009 15:44

Thanks Boris,

It makes sense now!
I changed the model to have atmospheric pressure on both inlets (Total Pressure = 101325 Pa) and flow rate of 160 mL/min on the outlet (80 mL/min for each inlet). This solved my problem of not knowing the pressure differential to get the correct flow rate.

Thanks again for the detailed and in depth explanation.
It certainly helped me!

christina2009 August 11, 2009 04:23

Quote:

Originally Posted by Eran (Post 222969)
Dear All,

I am working on simulating air flow in an existing model. The model has two air inlets and one outlet. The inlets are on opposing sides of the symmetrical model.

Currently I only know that 80 mL/min of air is coming from each of the inlets and of course 160 mL/min from the outlet. The air is pulled by creating a small vacuum on the outlet while the inlets are exposed to the atmospheric pressure.

Since I am new to Floworks I am encountering problems in setting the boundaries. I tried to set only flow boundaries on the inlets and outlet, however, I received an error message that the model has to have pressure boundaries to work. Since I don’t know the pressure differential between the inlet and outlet (I only know the air flow), this is a problem. I tried to set some arbitrary pressure in the inlet (you cannot set a negative pressure in the outlet), but I get some very high flows which do not make any sense.

My question: Is it possible to set only flow boundaries without pressure boundaries


thanks so much for useful info



All times are GMT -4. The time now is 01:14.