If the MFX solver is used and conservative interpolation is selected for the load transfer between CFX and ANSYS, the results can be incorrect although things appear to run fine.
When conservative interpolation is selected, the CFX variable name for the load transfer must be given as "Total Force" or "Wall Heat Flow", as documented in the ANSYS online help for the MFLC command. This applies whether the case is set up through the ANSYS Prep7 user interface (under "Custom" load transfer) or directly through the MFLC command in the ANSYS input file. If the CFX variable name is set up correctly, then cases where the conserved quantity (force or heat flux/flow) is transferred from CFX to ANSYS work fine and give correct answers, but cases where the conserved quantity is transferred from ANSYS to CFX will stop with an error as CFX is not currently capable of receiving "Total Force" and "Wall Heat Flow" quantities.
If the CFX variable name is given as "Total Force Density" or "Wall Heat Flux" for a conservative load transfer, then this is a setup error. However, the case will apparently run without errors. ANSYS will still send "Total Force" and "Wall Heat Flow" quantities, but CFX will read them as if they were "Total Force Density" or "Wall Heat Flux", which means that in effect, the received quantities are incorrect by an area factor. In most cases, this area factor will be sufficiently large that either the case will be impossible to converge or will converge to answers which are wrong by orders of magnitude and clearly incorrectly. However, for some cases the area factor may be close enough to 1 that apparently sensible answers can be obtained which are actually incorrect.
For cases where the conserved quantity (force or heat flux/flow) is transferred from CFX to ANSYS, ensure that the CFX variable is set as "Wall Heat Flow" or "Total Force" if you need to use conservative interpolation. For cases where the conserved quantity is transferred from ANSYS to CFX, you must use the profile-preserving interpolation option (default), with the CFX variable set to "Wall Heat Flux" or "Total Force Density".
ANSYS CFX 11.0.