Hi ,

I'm trying to plot some velocity profile graph in a adimensionless form so that I have to compute the average velocity in some sections of my problem (internal flow). Meanwhile, regarding some experimental data I have for the same experiment, it seems that FLUENT, when averaging the velocity in a section makes some numerical errors: indeed when comparing the flow rate after adimensionalisation with the experimental data it doesn't give the same results unlike it is obiously the case in the initial conditions.

Thanks for your help,

Andre.

I have made the same observation. If the mass flow rate is set on one inlet as bc. After calculation the mass flow rate is different from the value at inlet in report...surface integral...

jy

I've seen the same - "Report/Fluxes/Mass Flow Rate" does not give the same as "Surface Integral/Mass Flow Rate" on the same surface. Apparantly Fluent computes these two differently. The "Report/Fluxes" version is more correct and matches the boundary condition - ie, if possible, you should use this when you have a choice. The difference is bigger if your mesh is bad. Sometimes it can be as much as 30%. But most often it isn't very big.

For reporting fluxes on "boundary surfaces", "Report/Fluxes" gives the actual fluxes used in the finite-volume solver. The fluxes on the boundary surfaces are "stored", essentially at the faces of individual cells on the boundary surfaces and updated with the solutions. When you do "Report/Fluxes...", FLUENT merely retrieves the flux from the memory and display on your terminal. As such, the fluxes reported via the "Report/Fluxes" panel satisfy conservation laws (mass, momentum, etc.) and can be regarded as "solutions" themselves and therefore more "accurate" than "derived" quantities.

"Report/Surface-Integrals ..." is a different animal. It allows you to compute fluxes and integrals on arbitrary surfaces, not only boundary surfaces but also internal surfaces of your choice. However, the fluxes and integrals reported via this panel are "derived" quantities, not "solutions" in themselves. The fluxes and integrals ought to be "computed" by interpolating (for internal surfces) or extrapolating (for boundary surfaces), as needed, the solution fields which are stored "at cell centers". As a consequence, the fluxes and integrals reported via "Report/Surface-Integrals..." can't avoid interpolation and extrapolation error. For reasonably fine meshes with well-thoughout boundary surface locations, the "reporting error" will be small enough.

We have a plan to improve the "reporting" accuracy in "Report/Surface-Integrals" in the upcoming release.