Large space simulation
 

Dear all,

I met a problem in Large space simulation.

I simulate the outdoor airflow around buildings, and the domain height is about 100m height. Since I set the Gravity force to be constant, and Outlet external pressure 0 relative to 1E+05 pa.

Then the pressure stratified in the domain because of the height, and most of the area is negative pressure. That makes sense since the higher the position, the lower the pressure. Then the problem is the flow can not go out of the outlet, because the pressure inside the domain is lower than outside.

Could anyone help me with that problem?

Re: Large space simulation
 

Using the 'Constant' buoyancy model will generate a P1 field that contains the full hydrostatic component in addition to dynamic variations. P1 values in large scale external flows will therefore be larger at the bottom of the domain than the top: this is not consistent with the specification of a constant external pressure, and will often lead to severe flow distortion near the 'outlet' - flow out at the bottom and in at the top.

The usual approach is to use a different buoyancy model: 'Density difference' or 'Boussinesq' will effectively remove the hydrostatic component from P1. This usually enables a fixed pressure 'outlet' to be used safely (provided that the reference density or temperature is appropriate for the ambient conditions).

If there are good reasons why the 'Constant' buoyancy should be used, or if the P1 variation at exit still causes unacceptable flow distortion with the other models, it is often possible to solve the problem by reducing the Coefficient specified for the 'outlet': this will increase the difference between the in-cell P1 values and the specified external (to generate the necessary outflow) value, so some care is needed to ensure that the pressure within the solution domain does not become unrealistic.

Alternatively, it is easy to specify the external pressure as a function of height using In-Form (see POLIS for more information). This requires the object to be User-defined, with a PATCH (having the appropriate area type) associated with it; no COVALs should be created (unless there may be genuine inflow, in which case the Coefficient should be set to 0.0 and the Value to the appropriate external value).

Then an In-Form statement like (SOURCE of P1 at OUTLET1 is 1.0*(1.189*9.81*(50.0-YG)-P1) $ with IMAT<100!LINE)will impose an external pressure at patch OUTLET1 that is linear in y. The external pressure is 1.189*9.81*(50.0-YG), where 1.189 is the density at the ambient temperature, YG is the y-coordinate at the cell centre and 50.0 is the reference height for the pressure; this is the Value that would be used in a conventional COVAL setting and 1.0 is the Coefficient. IMAT<100 ensures that a source is only created in fluid cells and !LINE applies source linearisation; $ indicates that the statement is continued on the next line. Note: some pressure relaxation will usually be needed when In-Form is used in this way - linear relaxation of 0.3, perhaps.

John,

Re: Large space simulation
 

Sincerely thank you very much!

yazhuo