CFD Online Discussion Forums

CFD Online Discussion Forums (
-   CFX (
-   -   Is it a Bug with CFX 5.4 ?? (

Veebs November 24, 2001 05:44

Is it a Bug with CFX 5.4 ??
Dear CFX 5.4 users, I modelled a axisymmetric cavity using CFX 5.4. As adviced with manuals I have only one element in the theta direction. I compute the wall velocity components with following equations.

tomega = 2*3.1415*27634 /60 [s]

angle = atan(z/y)

radii = sqrt(z*z + y*y)

vttheta = tomega*radii

vzt = vttheta*cos(angle)

vyt = vttheta*sin(abs(angle)) I have taken both velocity components positive as the domain is in 2nd Quad.(I will get clockwise sense of rotation)

When we postprocess the results (using hybrid) based wall velocities are found to be computed based on angle evaluated at face average and NOT AT NODE. I have a 2Deg model. But angle comes as 1 deg for all the wall nodes (should be 2 or 0). Is this a bug with CFX 5.4 ? How to get rid of this problem ? ( I already posted a message here but no reply on this) Thanks for your time Veebs

P.Fonteijn November 25, 2001 18:15

Re: Is it a Bug with CFX 5.4 ??
I don't understand your your problem exactly. But for this kind of calculations I usually use atan2(z/y) in stead of atan(z/y). Maybe it helps.


VEEBS November 25, 2001 23:57

Re: Is it a Bug with CFX 5.4 ??
Dear Fonteijn

When we model with boundary conditions defined using experssion editor, Instead of using node based coordinates for expression calculations, It uses face center values. (Very easily checked with axisymmetric model with only one element in the theta direction)

Thanks for your suggestions. But it does not help.


Stuart November 27, 2001 09:54

Re: Is it a Bug with CFX 5.4 ??
Veebs, what do you get if you use the conservative results ? is there any difference ? stuart

Dan Williams November 27, 2001 16:50

Re: Is it a Bug with CFX 5.4 ??
Hi Veebs,

As you have surmised, the solver applies your inlet velocity boundary condition at the center of each element face on the inlet. So each control volume on the inlet boundary sees a different velocity on each integration point which contributes to the fluxes. The control volume values of the velocity will be solved for based on the velocities which are used to close the boundary condition on the surrounding faces.

The hybrid values for each node on the inlet are the arithmetic average of the element face values which surround the node on the boundary. Since the boundary conditions in CFX-5 are face based, a single node never really "sees" a single velocity, i.e, it's closed with inlet/wall/symmetry etc... (depending on how many boundary conditions surround it) so for the hybrid value you get an approximation which is set to the average.

If you ran with more than one layer of elements in the theta direction, say 3-4, you would see that some of the nodes on your boundary will actually have the proper values. In your case the nodes which lie on the intersection of the inlet plane and the symmetry planes behave as you mention.

Unfortunately there is no way to control this directly in the CFX-5 solver, and it's not clear what to actually do in general. It's not a bug, it's just a consequence of two competing requirements, i.e., how the control volume equations are discretised and what the boundary conditions actually are. So, we live with it to a certain extent.

One workaround you might try is create an new variable in CFX-Post or an algebraic additional variable in CFX-Build which is set to your expression so that you can plot exactly what you want to see.


VEEBS December 1, 2001 05:38

Re: Is it a Bug with CFX 5.4 ??
Hi Dan, Thanks for your view and I also accept that. I guess while modeling axisymmetric models with CFX 5, following should be recommended.

1. Go with minimum possible sector angle (theta)

2. Minimum of 3 elements in the theta direction to be used. And the results shall be taken from internal nodal planes.


All times are GMT -4. The time now is 05:41.