# Large space simulation

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 February 23, 2003, 23:25 Large space simulation #1 Yazhuo Qian Guest   Posts: n/a 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?

 March 27, 2003, 11:42 Re: Large space simulation #2 John Heritage Guest   Posts: n/a 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,

 March 27, 2003, 12:13 Re: Large space simulation #3 Yazhuo Qian Guest   Posts: n/a Sincerely thank you very much! yazhuo

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Emmanuel Kasseris CD-adapco 10 October 25, 2008 17:12 Shamoon FLUENT 0 April 20, 2008 02:39 Sheikh Tamjid Mashrafi FLUENT 2 February 4, 2008 15:39 Chungang Chen Main CFD Forum 4 January 25, 2006 06:09 Randheer Yadav FLUENT 0 July 27, 2005 16:38

All times are GMT -4. The time now is 23:53.

 Contact Us - CFD Online - Top