Hi Frienz,

My problem is mass flow in is not equal to mass flow out. In function calculator. AVE ,IN ,MASS FLow AVE ,out,Mass Flow Here the values of in and out is not same.

My problem is flow control valve condition : Reference pressure 0 bar inlet-openingressure and dirn-1.01325 bar outlet-openingressure and dirn-0.95 bar My valve is in full open condition Can anyone tell me why in is not equal to out.

Your simulation seems not to be fully converged. Some tips that might help:

1 - extend a bit you domain. Maybe your bondaries (mainly the out) are too close to the valve, in a region where the turbulence is too high. This may cause things like fluid entering your domain through the outlet. The BC should be placed, whenever possible, in a region where the flow profile "behaves better" (no eddys or strong curvatures in the streamlines).

2 - why are you using openings for the BC? normally using inlet and outlet makes the convergence easier.

3 - definning both BC by pressure is hard for convergence. It would be better to define velocity for the inlet and pressure only for outlet. If you dont have it, maybe you can guess a velocity profile (even if constant) just to have an approximated result and use it as initialization condition for you simulation. For sure it would be faster.

Skarp,

You may be calculating it wrong in CFX-Post. Use the massFlow()@location function only, calculating the sum of Density*Velocity*Area or anything else will return the wrong value (albeit only slightly) because they do not use the exact flows stored at integration point faces. But before you do this, check the flow summary in the OUT file, what does the solver report as the mass imbalance? You can also plot imbalance in the solver manager.

If the flow is incompressible, you should also specify your domain pressure as 1.01325 [bar] and then specify your boundary conditions relative to the domain pressure (i.e. 0 [bar] at the inlet and -0.06325 [bar] at the outlet). This may not effect you mass imbalance (if there is indeed an issue), but it will reduce round-off errors.

-CycLone

Hi cyclone

U r really perfect. My calculation in Function calculator is wrong. U r notion work out.Expression answer is accurate to my experimental result.

One thing i was confused is that What is the difference Given as massFlow()@location and massflow ave in function calculator.

Hi Skarp,

'massFlow()@location' returns the total mass flow through the location. 'massFlowAve(variable)@location' returns the mass weighted average of a variable at the location. Alternatively, you can look at it this way:

massFlow()@location = sum(Mass Flow)@location massFlowAve(variable)@location = sum(Mass Flow * variable)@location/sum(Mass Flow)@location

The expressions given above should return the same values. Area average is calcuated in a similar way but uses area as a weighting function.

-CycLone

Actually i have given in this manner function - ave location - in variable - mass flow

For all my problems normally this i used to give mass in = mass out But in valve control problem it is not equally. Can u tell me why ?

I do not recommend specifying the mass flow rate at both the inlet and the outlet as this would be overspecifying the problem. The solver is strongly conservative and if you specify a mass flow at one end and a pressure at the other, the net result will always be that the inlet mass flow is equal to the exit mass flow.

If this is not the case in your run you are either: i) not calculating mass flow properly in Post, or ii) the run is compressible and has not converged.

For incompressible flow the imbalance is reduced to well below 0.1 % within the first 10 to 20 iterations. Compressible flows may take longer because the domain pressure may change and mass will be accumulating (+ or -) within the domain.

So what exactly are you doing?

-CycLone

Sorry I mean is

in and out i give it as pressure.

In function calculator to find mass flow rate .i used to give function-ave,location-in,variable-mass flow

In the calculator for many problems the answer in the calculator to find the mass flow rate ,mass flow in and out are same.

but in flow control problem it is not same.

Hi. I am facing same problem of inlet and outlet massflow difference. In my steady state simualation there are two inlets and two outlets to an agitated tank. There is continuous aqueous phase and droplets of organic fluid are dispersed. Fluids separates by density difference- dispersed phase leaves at upper outlet and continuous phase from lower. At outlets I have defineed average static pressure with flow direction and at inlets mass flow rates.

Please give suggestions to specify physics and boundary conditions so that I can set this problems