Calculating flow through an area

 Register Blogs Members List Search Today's Posts Mark Forums Read

 April 22, 2009, 17:35 Calculating flow through an area #1 New Member   Mike Jenkins Join Date: Apr 2009 Location: Kansas City Posts: 9 Rep Power: 10 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.

 April 22, 2009, 17:37 #2 New Member   Mike Jenkins Join Date: Apr 2009 Location: Kansas City Posts: 9 Rep Power: 10 also see this forum I posted to calculate the velocity: http://www.cfd-online.com/Forums/cfx...html#post91803

 April 22, 2009, 20:27 #3 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,805 Rep Power: 107 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

 April 25, 2009, 05:11 #4 New Member   Join Date: Apr 2009 Posts: 2 Rep Power: 0 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

 April 26, 2009, 19:07 #5 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,805 Rep Power: 107 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

May 1, 2009, 13:39
averaged massflow
#6
New Member

Join Date: Mar 2009
Posts: 8
Rep Power: 10
Quote:
 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

 May 2, 2009, 08:45 #7 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,805 Rep Power: 107 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

May 12, 2009, 13:26
how to create an evalation plane
#8
Member

Jules Bell
Join Date: May 2009
Posts: 31
Rep Power: 10
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
Attached Images
 slot.GIF (26.3 KB, 41 views)

 May 12, 2009, 18:50 #9 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,805 Rep Power: 107 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

 September 11, 2009, 15:34 Solution! #10 New Member   Mike Jenkins Join Date: Apr 2009 Location: Kansas City Posts: 9 Rep Power: 10 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.

October 19, 2012, 11:31
#11
Member

Join Date: Jan 2012
Location: Indiana, USA
Posts: 84
Rep Power: 7
Quote:
 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?

 October 20, 2012, 05:27 #12 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,805 Rep Power: 107 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.

January 17, 2017, 10:17
#13
New Member

Tobias Hanisch
Join Date: Nov 2014
Posts: 2
Rep Power: 0
Quote:
 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.

 January 18, 2017, 04:28 #14 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,805 Rep Power: 107 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 likes this.

 January 18, 2017, 06:17 #15 New Member   Tobias Hanisch Join Date: Nov 2014 Posts: 2 Rep Power: 0 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: CFX-Post: problem with mass flow )! Antanas, fresty, -Maxim- and 1 others like this. Last edited by hanischt; January 18, 2017 at 07:18.

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Nitin FLUENT 9 June 17, 2017 10:30 make OpenFOAM Running, Solving & CFD 2 October 16, 2007 05:47 diaw Main CFD Forum 104 February 16, 2006 06:44 Paul CFX 2 August 11, 2003 09:41 Adrin Gharakhani Main CFD Forum 13 June 21, 1999 05:18

All times are GMT -4. The time now is 21:17.