CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   CFX-Post: problem with mass flow (http://www.cfd-online.com/Forums/cfx/20969-cfx-post-problem-mass-flow.html)

Markus February 3, 2005 22:05

CFX-Post: problem with mass flow
 
Hi!

My problem is that I need to calculate the mass flow at different cross sections in my fluid domain. The calculator always gives me a mass flow of 0 kg/s at planes that I have created in CFX-Post. The calcultion for boundary surfaces is no problem.

Then I tried to use to creat an expression: areaInt(Velocity*Density)@plane This expression gives me a value but I tried this expression at my outlet were I can use the calculator as well.

The calculator gives me the value of my boundary condition (-5e-005 kg/s), with the expression I get 3.78595e-005 [kg s^-1]!

Can anyone tell what is wrong and why the calculator is not working for the mass flow at created planes??

Thanks,

Markus

Rui February 4, 2005 15:38

Re: CFX-Post: problem with mass flow
 
Hi,

The calculator gives the value 0 kg/s, probably because you have defined the Plane Type as Sample, and the plane bounds are larger than your domain. Visualize the plane and see if it is larger than your domain.

If you define the Plane Type as Slice, the plane will be bounded by your domain size and I believe the calculator will give a value for the massFlow.

Note that your expression is not totally correct, as the massflow is correctly expressed by areaInt(Density * Velocity dot n)@Plane, where Velocity is the velocity vector, n the plane outward normal vector and dot indicates the dot product between 2 vectors. In your expression, Velocity is interpreted by the calculator as the velocity vector norm, and the result will be greater than the correct one (the results will be the same only if the velocity vector and the n vector have the same direction at every point).

The reason why the calculator gives a higher result for massflow than for your expression may be the same stated here: http://www.cfd-online.com/Forum/cfx.cgi?read=9519

Regards,

Rui

Markus February 8, 2005 17:26

Re: CFX-Post: problem with mass flow
 
Hi Rui!

Thanks for your help. I tried the expression but I recieve the following error message:

ERROR Error in setting: "mymassflow" via the expression: areaInt(Density*Velocity dot n)@Plane areaInt(Density*: read successfully, and then error found at item: Velocity dot n unrecognised name

The plane is defined as Slice.

Thanks,

Markus

formercfxuser February 9, 2005 16:17

Re: CFX-Post: problem with mass flow
 
Is one of your velocities normal to your outlet or the planes you want to investigate - then you could use that one. Even if that is not the case you could transform the velocities and create a variable wich is the normal velocity to the plane.

Rui February 12, 2005 16:18

Re: CFX-Post: problem with mass flow
 
Hi,

You receive that error because there isn't such variable "Velocity dot n". I meant that the mass flow through a surface is calculated as the integral of (density * Velocity DOT n) over that surface, where Velocity is the velocity vector, n the surface outward normal vector, and DOT is the dot (or inner) product between 2 vectors. You may find this in any fluid mechanics book.

CFX-Post doesn't do the dot product between 2 vectors. So, you have to do it by yourself. You have to create an expression: velDOTn=Velocity u*Normal X + Velocity v*Normal Y + Velocity w*Normal Z ; then create a variable, called NormalVelocity for example, and chose the expression VelDOTn.

To obtain the mass flow through a surface (which may be a plane or not) just do: areaInt(Density*NormalVelocity)@Surface

However, as stated in http://www.cfd-online.com/Forum/cfx.cgi?read=9519 , there may be a difference between the values obtained with massFlow and with the expression.

Regards,

Rui


Markus February 19, 2005 18:30

Re: CFX-Post: problem with mass flow
 
Thanks Rui! Seams to work well.

Markus


All times are GMT -4. The time now is 14:28.