[i621148]

What is the consensus opinion on how to calculate leakage through an area? I have tried calculating the cross sectional area and then multiplying by a measured velocity point in that area but since some areas are high proportionally to the rest of the area, the answer is not correct.

I have also tried graphing flow but it is not always constant in the areas either. Is there a way to calculate average velocity of an area or something and then multiply by the area?

Any other suggestions are welcome. I am trying to calculate a leakage rate through a crack.

[i621148]

also see this forum I posted to calculate the velocity:
http://www.cfd-online.com/Forums/cfx...html#post91803

[ghorrocks]

Hi,

In CFX you should use the massFlow() CEL expression to calculate the mass flows. Then it will correctly account for the integration points which your simple area times velocity approach does not. In most cases the difference should be small though.

Glenn Horrocks

[delalidei]

Hi,

If you create a 2D region at this area, you should be able to calculate the area averaged massflow through this area in CFX post. You need to create a table, then what you should enter is

areaAve(massflow) @ (region)

Delali

[ghorrocks]

Hi,

I suspect he is looking for the total mass flow, not the massflow per cell. In this case you don't use the areaAve() function, but should use the massFlow() function instead.

Glenn Horrocks

[ahlo7]

Originally Posted by delalidei

Hi,

If you create a 2D region at this area, you should be able to calculate the area averaged massflow through this area in CFX post. You need to create a table, then what you should enter is

areaAve(massflow) @ (region)

Delali

To created a 2D region in CFX Post?
I also want to get flow rate through a section of a tunnel, but I did not figure out how to make a 2D region at a section interested without including the flow outside of the tunnel.

Thanks

Ahlo

[ghorrocks]

Hi,

A plane can be defined to have bounds. Have you tried that? And as I mentioned previously use the massFlow() function to get the massflow directly on your surface.

Glenn Horrocks

[Jules]

Hi,

I have pretty much the same problem. I have a fluidic actuator cavity that is connected to the outside flow with a thin slit, as can be seen in the attached picture. One wall of the cavity is moving (piezo disc), so there is flow going back and forth through the slit. I would like to monitor the mass flow (in fact, the average velocity) and would like to use a CEL expression for that. However, there is no region defined that crosses the slit.
Is it possible to create a plane that crosses the slit in CFX Pre? Or do I have to define it in ICEM when creating the mesh? Doing it later in Post isn't really what I like, because then I can't monitor the expression during the solver run.

Thanks for your help!

Jules

[ghorrocks]

Hi,

I think you can do this in V12 but I am not sure.

In V11 or earlier you have to cut the mesh and reconnect it with an interface, preferably with a 1:1 connection. Then you have a surface to calculate the massflow rate on.

Alternately you can define a monitor point in the middle of the passage and monitor the velocity. Of course this is not the mass flow but sometimes it is enough and you don't need to remesh this way.

Glenn Horrocks

[i621148]

I have found that the best solution for my particular problem is quite obvious...

I used the massflow calculator as suggested to get the total flow but found that you can get the exact same result from clicking on the report generator (include default template).

A table of mass flow will then be given for each inlet, outlet and opening in the report preview window along with other useful information.

[Torque_Converter]

Originally Posted by ghorrocks

Hi,

In CFX you should use the massFlow() CEL expression to calculate the mass flows. Then it will correctly account for the integration points which your simple area times velocity approach does not. In most cases the difference should be small though.

Glenn Horrocks

Sorry to bring this up again but I am unsure if the CEL function massFlow()@interface... gives mass flow moving only in one direction or the total flux. The reason I'm thinking its just measuring everything going thru at any direction is the mass flow at these interfaces I am measuring is much greater than the mass flow entering the system or leaving the system near this interface. This region is highly turbulent with much recirculating flow since there are two different domain speeds. I also noticed you cannot definite an axial or any direction for this massFlow function. Is there any way to find out how much is passing into and out of this domain, and only the amount that moves on "forward" toward the exit?

[ghorrocks]

I have not checked but am pretty sure massflow gives the total flux, so it can go positive or negative. If there are regions of both forward and backward flow it will return the net flux (forwards-backwards).

Of course you do not define a direction for massflow - it is simply the massflow across the surface.

Not sure how you could split the flow into forward and backwards components. It is simple if your surface is flat, but if curved it is a bit trickier.

[hanischt]

Originally Posted by ghorrocks

Not sure how you could split the flow into forward and backwards components. It is simple if your surface is flat, but if curved it is a bit trickier.

Sorry to dig out this thread after a long time. I have the same problem as Torque_Converter. I want to evaluate the mass flow at an interface with strong recirculation, where I need to know the portions of mass flow going into and out of the domain.

Glenn, you said that it is easy to split the flow for a flat surface. But how would I do that? I already defined a monitor massFlow()@myInterface Side 1, but as expected I only get net flux.

Any help would be appreciated.

[ghorrocks]

Actually, this might be simple. But I am holidays at the moment so cannot look this up to check it correct.

If you get the absolute value of the normal component of the velocity at the interface (dot product with the face normal). If you areaInt() this function over the interface it will give you the flow in one direction. Take the negative of the normal component to get the flow in the other direction.

[hanischt]

Thank you for this push in the right direction!

After going through some other threads about the dot product, I finally found a way to solve my problem. Here's what I've done:

1.) Create an expression "VelDOTn" that calculates the dot product of velocity:

VelDOTn = (Velocity u*Normal X + Velocity v*Normal Y + Velocity w*Normal Z)

2.) Create a variable, called "NormalVelocity" and chose the expression VelDOTn

3.) Create three more expressions for forward, reverse and net mass flow:

mf forward = areaInt(Density*step(NormalVelocity / (1 [m*s^-1])) *NormalVelocity)@IF Side 1
mf reverse = areaInt(Density*step(-NormalVelocity/ (1 [m*s^-1])) * NormalVelocity)@IF Side 1
mf net = mf forward + mf reverse

The step function guarantees that only positive (or negative, respectively) values of NormalVelocity are integrated. Otherwise the expression again will only yield the net massflow.

4.) Comparison of the value of "mf net" with built-in function massFlow()@IF Side 1 shows very good accordance (0.00133908 [kg s^-1] to 0.00134141 [kg s^-1] means 0.174% deviation)

Thanks to Glenn and Rui (who explained how to use the dot product in CFX in another post: CFX-Post: problem with mass flow )!

[dboss]

Originally Posted by Jules

Hi,

I have pretty much the same problem. I have a fluidic actuator cavity that is connected to the outside flow with a thin slit, as can be seen in the attached picture. One wall of the cavity is moving (piezo disc), so there is flow going back and forth through the slit. I would like to monitor the mass flow (in fact, the average velocity) and would like to use a CEL expression for that. However, there is no region defined that crosses the slit.
Is it possible to create a plane that crosses the slit in CFX Pre? Or do I have to define it in ICEM when creating the mesh? Doing it later in Post isn't really what I like, because then I can't monitor the expression during the solver run.

Thanks for your help!

Jules

Sorry to bring this old topic up again.


I have exactly the ame problem.

Did you Jules or somebody else figure out how to create a plane across a certain fluid channel without cutting the mesh and create a surface for massflowaverage observing?
Thank you very much in advance.

[hanischt]

I doubt this is not possible. I would always create that plane in the mesh. You are not able to create a plane in CFX-Pre like you would do in Post.

[Jules]

Wow, this is from forever ago...
I can't remember whether I found a solution to this back then. I looked into the few CFX setup files from this project which I could still find on my hard drive, but there was no such monitor point for mass-flow, and no specified 2D mesh location where I would have evaluated the mass-flow, so apparently I gave up on that back then.
I haven't worked with ICEM since, so I'm not more knowledgeable in that regard than 10 years ago.
I know, however, from working with Turbogrid, that it is possible to have 2D mesh locations separating 3D mesh regions (i.e. grid blocks) within a single mesh domain, meaning that no interface is required.
My bet would be to create a planar surface at the location where you want to monitor the mass-flow ICEM, split the grid blocks at that surface and associate the corresponding block faces with the surface. Maybe that is enough to create a 2D mesh region at that location. If not, you may indeed have to create separate mesh domains and connect them with a 1-to-1 interface.
Hope this helps.