Mass flow calculation
 

I am solving a problem in which the flow goes into and out of a single defined surface. Please see the screenshot. Since there is no boundary between the regions that the flow goes in or out in the surface, CFD Post shows that the mass flow is zero at the surface.

Is there a way to estimate the mass flow that goes in/out seperately?

I was thinking that if I could use a conditional statement in which areaInt (density*velocity) is positive it should show the mass flow in one direction and if it is negative it would show the other mass flow.

Is is correct?

It depends if the velocity that you show is aligned with the global coordinate system. If so, then you can calculate the massflow in Z-direction as

UpwardFlow = areaInt(max(0[m/s],Velocity w))@Surface
DownwardFlow = areaInt(min(0[m/s],Velocity w))@Surface

If correct, than Upward and Downward flows are equal.

For X and Y take velocity u and velocity v

No they are not aligned.

Since the surface is annular and according to the definition normal velocity to the surface should be used to evaluate mass flow, should the radial velocity be used instead?

Should the area integral be evaluted over the projected area of the anuular surafce?

If the surface is annular, then in Post you should go to the Turbo Tab and let Post calculate the radial and tangential components. Then use the expressions given above and use "Velocity Radial" in stead of Velocity w.

How about the surface? Should the projected area normal to the veocity be taken or the annular surface itself?

I would take the annular surface..
If you have any doubt, calculate all numbers that you might think are relevant and try to understand what they mean and if the result makes sence. In that way you learn what Post is calculating.
In principle there should be a mass balance: all fluid going upward should equal to the fluid going downward, except for the flow towards inlet and outlets.

If you are using a surface that is not an external boundary, the Normal vector is not well defined, i.e. arbitrary side of the surface. If so, first order of business is to know what is the Normal direction used by CFD-Post, i.e. create a vector plot on that surface of Normal.

With that out of the way, the next step is to compute the mass flow correctly,

Net_massflow = areaInt (density * VdotN)@surface

VdotN = Velocity u * Normal X + Velocity v * Normal Y + Velocity w * Normal Z

Two down, two more to go.

SignedP_massflow = areaInt(density * max(VdotN, 0))@surface

SignedN_massflow = areaInt(density * max(-VdotN,0))@surface

I think that should do what you want. Keep us posted..

PS: Using density * velocity, you are using the magnitude of velocity as far as I recall

Thank you for your replies.
Similarly, I would like to calculate the averaged-circumferential velocity of the flow going inside/outside the surface seperately.
Is there a way to limit cfd post to calculate the velocity seperately in a single surface where flow goes inside/outside? Please see the screenshot in the first post. They are normal velocity vectors to an annular surface.

You could try to create an isoclip in CFD-Post of the same surface, limiting it to the directional velocity in the desired direction (greater or smaller than 0), and then calculate massFlow on this clip surface.