Hi all:

I am modelling isothermal flow of air in a room with one inlet and one outlet. The grid I am using is cartesian and uniform at the inlet and outlets.

When I ask CFX to export the mass flow rates at the outlet and I sum these individual mass flows they equal approximately 0.602 kg/sec which is the same as the inlet and a mass flow balance is achieved.

However, when I multiply the individual velocities densities and areas (pVA) at the outlet and sum these totals up for the outlet, the total is only 0.560 kg/sec.

Can anyone explain to me what CFX is doing?

Thanks

Jeff Berg M.Sc. Student University of Manitoba

Hi Jeff,

The solver calculates mass flows for each element sub-face. On a hex element face at a boundary, there are four sub-faces. CFX-Post will account for this when calculating mass flow, but your expression will not. This is actually a good reason to use CFX-Post for quantitative post-processing over third party post-processors, since they do not account for the discretization used in the solver.

Have a look at the discretization theory in the documentation for more information.

Regards, Robin

I have also the same problem, on the descritisation section of the manualit says variables at the faces are calculated by multiplying the weighted distance by adjusant cell centers w.r.t the face, however it is not working for me. Just I am puzzled

i am not sure i am right .. but i suspect this might be related to this issue: at the out let , to accelrate convergence , after every iteration the total sum is calculated and then based on the inlet massflow, the flow factor is caculated .and that is the mass imbalance, then all the values at outlet are multiplied by this flow factor so that it matches with the inlet flow. (this helps in fast convergence), so if you see at the dummy cells of outlet the mass flow sum should be equal to inlet (as it is adjusted), but if you calculate it based on velocites and area, it will eb different and less at the outlet.

(i am only guessing but this might be the reason)

Dear Fluent user,

That is a common approach with segregated solvers (I don't specifically know what Fluent does, so you may want to check your documentation), however CFX-5 doesn't need to do any artificial adjustment of the outflows to match the flow rate. Rather, the coupled-multigrid algorithm will rapidly communicate changes through the domain. The actual mass flow out of a pressure boundary condition is based only on the local conditions and the pressure specified.

In a compressible flow simulation, the difference in inflow vs. outflow is balanced by the change in holdup within the domain (due to change in density). In equation form:

mass flow in = mass flow out + mass accumulated

If the flow is incompressible, mass cannot be accumulated and generally the mass imbalance will be reduced to round-off with the first 10 to 20 iterations.

Regards, Robin

humm, well , this is true that i never worked with cfx 5. so i don't know about how it does, so what you said about it , i assume is correct, that people who use cfx 5.7 are using coupled solvers. further about fluent, in their manuals ..its not very clearly mentioned ..fluent manuals are not as good as cfx's manuals (i worked with cfx 4.3 , 4.4)