Drag force on cylinder (laminar flow)
 

Hello,

I've been trying to get the drag force and from there the coefficient of drag force yet I have this warning:

WARNING
Unable to calculate mass flow for the surface.
Some or all of the required variables are not present:
Density; Velocity; and for multi-phase cases, Volume Fraction.
Do I need to define the values for these variables in CFD-Post or CFX-Pre?
Also when I look into force in the variables list it shows that it is unknown. Why could that be the case?
Thanks in advance!

Do you get this message in the solver or the post processor?

I get the warning in the post processor, and have tried to calculate force with various inputs of expressions with different surfaces yet it fails to give me an answer.

I just tried again, this time in CFX-Pre, with force_z, Normal Z and areaave(force_x) and I get the error:

"The following unrecognised names were referenced: areaave, force_z."
I would really appreciate if you could help, thanks!

Post #3: Then you did not include this data in the results file. Some required variables are not present.

Post #4: The function name is "areaAve". force_z should work. The full list of functions, variables and their correct syntax is the CFX documentation in the reference guide.

The expressions are chase sensitiv. Try force_Z

1) Where can I have access to the results file, I remember I selected some variables but I forgot where I accessed them...

2) after I get the results with the streamline, I am trying to get the data from one of the point, or line to get the recirculation bubble length in the wake of the cylinder yet I am unable to pinpoint which point/line/plane I should pick to derive the graph of axial velocity against length. Any suggestions?

Thank you so much for your help ghorrocks and Chris_321!

You defined the variables to go in the results file in the output tab of CFX-Pre. Unless you really need to save space I usually put all variables in the file to avoid this exact situation.

Precise definition of recirculation sizes is not a simple thing in 3D. In 2D it is straight forward as the location where the flow splits is the recirculation point, but in 3D you often have a flow in the third dimension - so is that in or out of the recirculation? So in 3D often you have to come up with some form of definition of recirculation size which is specific for your case. If could be where the axial velocity reverses on a central plane, or the wall shear stress reverses, or what streamlines from that point do.

Thanks for your reply ghorrocks. I have tried what you suggested and included all the variables in the output file yet I still have a problem:

For force_z()@cylinder (in CFX-Pre) it gave the following error:

ERROR
Attempt to evaluate the CEL callback function 'force'.
Although it is valid to create an expression that
uses such a function, the preprocessor does not support
its evaluation

Then I tried force_z(t)@cylinder (since it is a transient flow and I want to plot the graph of oscillating drag force values against time)
But I again get an error this time it is the following:
ERROR

In the expression assigned to 'expression', the function 'force_z' is called with the wrong number of arguments (1 - expected 0).

Thanks again in advance!

force_z()@cylinder is correct. The solver should be OK with it. The pre processor does not accept the full range of CEL expressions.

force_z(t)@cylinder is wrong, as the error message says. It does not use an argument.

You can use the chart function in cfd post for the transient plot of the Expression.