Learning Forum

[Sergio92]

I am using ANSYS 2020R1 to simulate laminar flow around a spherical obstacle. I have chosen an axisymmetric domain, so my sphere is represented as a semi-circle next to the symmetry axis x. Simulations are run using Fluent, and all the files (geometry, mesh, case and post) are managed from the Workbench. My simulations contain a scalar representing solute dissolved in the fluid.nAfter I run a simulation, I wish to compute the force exerted by the solute on the sphere. This force comes from solute-sphere interactions at a distance, and I calculate it by integrating a volumetric force f over my domain.nn#######################################nUsing Reports Definition in Fluent to calculate the integralnSum(f * 2 * PI,['corps_surfacique'],Weight = 'Volume')nI get 6.7558829e-14 Nn#######################################n#######################################nUsing Function Calculator in CFD-Post to calculate the integralnFunction: volumeInt; Location: corps_surfacique; Variable: fnI get 6.91156e-14 Nn#######################################n nNow I know these values are quite close. But this small difference affects my end results significantly. The field function f depends on scalar and position, so I have tried doing some things to figure out the exact reason for my issue.nn1) Integrating the scalarnResults are the same in Fluent and CFD-Postn2) Integrating abs(x)nResults differ by only 0.0084%n3) Integrating abs(y)nResults differ by 0.45%n nMy guess from these outcomes is that mesh elements in Fluent and CFD-Post have slightly different coordinates. Is that correct? In any case, which option should give me the most accurate result: Fluent or CFD-Post?n

[Rob]

Fluent is most accurate. CFD Post originates from CFX and is node based, Fluent is cell based. As you note the differences are small, and as you further refine the mesh disappear. Note CFD Post is not inaccurate, the difference is the result of the data interpolation rather than precision. n

[YasserSelima]

In your expression, Why are using 2*PI? n

[DrAmine]

Read about the limitations and differences when reading Fluent results into CFD-Post. Please rely on the Fluent Results.nn: 2D axis symmetric case.n

[YasserSelima]

my understanding is that fluent calculates the cell volume by rotating the 2D cell. So, why 2*pi!!n

[YasserSelima]

I got it, reference is 1 rad!n

[Sergio92]

Yasser:yes, you got it right.Thank you, Rob and Amine, for your prompt replies! That answers my question.nIf I may be just a little nitpicker:your answers were marked as accepted without me doing so. (I would do it anyway, so it doesn't really bother me)n

[DrAmine]

As you like.n