Hello everyone! I want to set velocity in some places in compuational domain in CFX5. How can I do it? What I want is that set the velocity in some points to be zero. I know it is easy in CFX4 but how to do it in CFX 5? It is very difficult to converge in CFX4. Thank you very much!

Hi cfxbeginer,

There is a FAQ on the CFX5 community website which describes how to do this.

http://www.software.aeat.com/cfxcommunity/

Glenn

Can you post it? I can not visit that website. Thank you very much!

Thank you very much!

or you can send it to my email address: yydcfdynamics@yahoo.com Thank you very much

You could also ask for a login code at the CFX helpdesk. That would be a lot easier.

Astrid

Hi,

I have copied the text here for all to see. Hopefully ANSYS/CFX does not have a problem with the copyright infringement! As Astrid said, I highly recommend you get a login on the site yourself. There is a lot of other useful stuff there.

Note that the example is for a scalar variable, but the principle should be able to be used for a momentum source to fix a velocity to a certain value. Also it lost the formatting in the copy/paste, but hopefully you can work it out.

Glenn

*****

The following explains how to maintain a scalar variable equal to a chosen value whilst it is transported (calculated) elsewhere. The proposed method creates a point source (using extra ccl) and sets the following source expression for the variable:

S = Scoeff x (Transported_Value - Specified_Value)

where:

Scoeff = negative value which is large compared to the convection and diffusion terms.

Below is the CCL example used to define a source expression that maintains a scalar value equal to 1.0 kg/m3 at the location of (1.0, 0.5, 0.5)

LIBRARY : CEL : EXPRESSIONS :

scoef = -100.0[s^-1]

svalue = scoef*(scalaire - 1.0[kg m^-3]) END END ADDITIONAL VARIABLE : scalaire Option = Definition Variable Type = Volumetric Units = [kg m^-3] END END FLOW: DOMAIN : scalar SOURCE POINT : I1

Option = Coordinates

Coord Frame = Coord 0

CARTESIAN COORDINATES :

X = 1.0 [m]

Y = 0.5 [m]

Z = 0.5 [m]

END

FLUID : Air at STP

SOURCES :

EQUATION SOURCE : scalaire

Option = Source

Source = svalue

Source Variable List = scalaire

Source Coefficient List = scoef

END

END

END END END END

Note that:

It is critical that the coefficient that multiplies the transported value, in this case "scalaire", has a negative coefficient. The source term can only be "linearized" automatically inside the solver if it is a negative coefficient. If a value of Scoef = + 100 was used, the converged answer would be basically identical (e.g. scalaire = 1.0), but the path to convergence would be much worse, because the source term would not be linearized. In the case of a "real" source term, all physical source terms that depend on a variable have "negative dependence" in order to keep the source term feedback finite (physical explosions have a positive feedback coefficient...).

The source term must be "large" relative to the flows through the local control volume equation. For example, for an advection dominated flow on a uniform grid you could estimate the mass flow through a typical control volume (density * velocity * area, where area = area of c.v. face = (c.v. length * c.v. length). The advection flow of a scalar from this mass flow is "mass flow * phi". The coefficient "Scoeff" will have the same units as mass flow for this simple example, so if you make Scoeff 10 times the mass flow rate, then this should be "large enough".

An easier way would be to do a run without the source term. Look at the inlet and outlet flows reported at the bottom of the out file for the transport equation of interest. Compute an "Scoeff" such that:

[Scoeff] = S / Phi_spec

where S is a source term of the same order as the inlet or outlet flow. This should be a very large source value, especially if it is used at only one location.

This can used to match a measurement for example. Examples of applications are for concentration of pollutant or temperature.