CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   CFX (https://www.cfd-online.com/Forums/cfx/)
-   -   Calculating flow through an area (https://www.cfd-online.com/Forums/cfx/63885-calculating-flow-through-area.html)

 i621148 April 22, 2009 17:35

Calculating flow through an area

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 April 22, 2009 17:37

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

 ghorrocks April 22, 2009 20:27

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 April 25, 2009 05:11

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 April 26, 2009 19:07

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 May 1, 2009 13:39

averaged massflow

Quote:
 Originally Posted by delalidei (Post 214142) 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 May 2, 2009 08:45

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 May 12, 2009 13:26

how to create an evalation plane

1 Attachment(s)
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.

Jules

 ghorrocks May 12, 2009 18:50

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 September 11, 2009 15:34

Solution!

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 October 19, 2012 11:31

Quote:
 Originally Posted by ghorrocks (Post 213837) 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 October 20, 2012 05:27

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 January 17, 2017 10:17

Quote:
 Originally Posted by ghorrocks (Post 387631) 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 January 18, 2017 04:28

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 January 18, 2017 06:17

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:
Code:

`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:
Code:

```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: https://www.cfd-online.com/Forums/cf...html#post70978)!

 All times are GMT -4. The time now is 08:30.