I am trying to model the air flow and heat transfer within a rectangular plant room with the following conditions:

- An rectangle inlet (protruded) located at high level with constant inlet velocity and air properties

(supply from a HVAC duct) - An rectangle outlet (protruded) located at high level at the opposite end (exhaust to open air) - Some machines simplified as rectangular blocks on the floor with constant heat flux - Steady state condition with the Temperature equation turn on

In STAR-DESIGN, I assign "NORMAL INLET" (at 25-deg C) boundary properties to the inlet surface, "OUTLET" to the outlet surface, all other wall are set at 33 deg C.

When I try running the solver (using tetrahedral element), the following error message appear:

*** ERROR #064 *** FIXED VELOCITY BOUNDARY

CONDITION OUTFLOW EXCEEDS INFLOW BY 5 PER CENT.

CONTINUITY CORRECTION NOT ATTEMPTED; EXECUTION

STOPPED.

Some user has suggested previously that refining the mesh can solve the problem.

Then I reduce the triangle size of the inlet and outlet boundary from 0.35 to 0.1. The global mesh properties was kept constant at 5%. The mesh size of the inlet and outlet surface looks finer but still got the same error.

Physically, the ouflow quantity will match the inflow quantity automatically by continuity.

Is there any other methods to resolve this problem? Should I change to outlet surafce to a "PRESSURE" boundary condition and give it the value of atmospheric pressure? Or can we change the 5% discrepancy limit to a higher value so that the solver can apply the continuity correction?

Don't use the "fixed velocity" switch for inlets. Using a pressure for the outlet is always a good idea.

You have "Inlet" boundary conditions assigned to both the inlet and the outlet. The specified mass flow through the inlet must exactly match the flow through the outlet to satisfy continuity. The mass flow through these as you have defined it does not balance.

Change the boundary condition on the outlet to "Outlet" with flow split 1.0.

Sorry to differ with Jorn, but using Pressure boundaries should only be used when you have to for some reason - they can cause instability, divergence and weird results if you're not very careful with them. Inlet/Inlet and Inlet/Outlet BC combinations are far more stable and represent a better defined problem.

Increasing the 5% discrepancy limit will simply break the continuity equation, and give you garbage results.

I have figured out the cause now.

I made the model and assigned the region's boundary condition in STAR-DESIGN by mean of additional file. Then I tried check the model in Pro-STAR and found that the regon # in Pro-STAR and STAR-DESIGN are different.

By changing the region# to the one used in Pro-STAR, the problem is solved, the solver be be started and get a reasonable solution.

The outlet boundary condition is still using the simple OUTLET option.