[LBOstudent]

I'm completing a university coursework in Phoenics. I have to model buoyancy driven ventilation for a school building. 3 floors, each with 20 students connected, to a central atrium.

People and computers have been modelled as computers and desks as plates on the horizontal plane. I have applied only the convective component as the heat from people and computers and applied the radiant fraction to plates (downward) on each ceiling. Openings have been placed on walls and the roof of the atrium and calculated based on the predicted NPL.

1. Should I be using flair or core? What's the difference?

2. What is the correct object to model computers? (I'm using people)

3. I used seated people for my intial run before deciding this probably too complex. I then replaced them with simple cuboids and my simulation is taking hours longer. How can this be!?

4. I need to demonstrate a grid sensitivity study. Can I create a "tailored mesh" and increase its density using the auto mesher? Or will this replace my mesh with a generic one? Should this be just a study of mesh density?

5. I have located the probe near an opening, on the middle floor. Is this a suitable location? My understanding is this should help me converge more quickly.

Any help would be hugely appreciated as no support is available over Christmas. Many thanks!

[phoenics_cfd]

PHOENICS-FLAIR is to be preferred over core PHOENICS for this type of application because there are a large number of input and output features specifically targeted for this type of application ( see http://www.cham.co.uk/phoenics/d_pol...r313/tr313.htm )

When modelling the heat sources from the occupants of a room, there are a number of factors requiring consideration and the modelling decisions depend on what is required from the simulation. However, it suffices to say that we usually make the following simplifying assumptions are usually made: (a) Breathing is not simulated. (b) the heat is put directly into the air, not into a solid. (c) The person is not represented as a solid blockage; instead, it is regarded as a region of air into which the heat is put. (d) If there are more than a few people representing heat sources, we usually distribute the heat sources over a rectangular region of air, of suitable size and location. (e) If there are only 1 or 2 people representing heat sources, we might specify individual heat sources where the people are located. But we still put the heat directly into the air, not into a solid. The people are not therefore "blocked".

In FLAIR, heat sources from people may be specified in a number of different ways, as follows.

(a) Use a domain-material Blockage to represent a rectangular region over which the heat source (perhaps representing several people) is to be distributed, and specify the appropriate heat source for the Blockage.


(b) As (a), but use a "People" object to specify a similar rectangular region, over which the heat source is to be distributed. Note that this object type allows you to specify a heat source, and nothing else. The object is not blocked. The default shape for a "People" object is "crowd"; this is rectangular (like a "cube"), and appears pink and transparent in the VR Editor. Note that a "People" object, unlike a "Blockage" object, does not specify a material type; this can be advantageous in certain situations.


(c) Use a "Person" object to represent the heat source for an individual person. By default this puts in 58W (which can be changed) over a "standing" person-shaped region of air. Note that the benefits of using this detailed shape are in all probability highly illusory, since the fine geometrical details of the "standing" person's shape will not be captured unless a very fine grid is used.


In general we would use method (b), although method (a) is essentially very little different.

The location of the probe will have no impact on the convergence of the solution. It is best to locate the probe in a region of flow sensitivity.
If you are having problems with convergence, you can read the lecture about convergence in POLIS. It is well written, and addresses most of the important points. It can be found here:

http://www.cham.co.uk/phoenics/d_pol...s/converge.htm.

Incidentally, the solver can display convergence-monitoring information on the screen as graphs of:

• Spot values and sum of absolute residuals vs. sweep (the default, described above),
• Maximum absolute correction and nett sum of sources vs. sweep,
• Minimum and maximum field values vs. sweep.

The selection is made in "Menu" / "Options" / "Monitor graph style", and can be changed in mid-run by "clicking a character key to interrupt"; then clicking the blue "Monitor" box at top right; and finally clicking the "Mode" button. Probably the most informative of the additional information that can be accessed this way is the maximum absolute corrections to the variables. In effect, these represent the maximum change in a variable over the whole domain. Once the largest correction falls to zero, or at least a negligible fraction of the value being corrected, it would be reasonable to assume that convergence has been achieved, even if the sum of the residuals has not fallen below any specific level.



I have run out of time now, but in any case it is difficult to advise any further without looking at your model set up. If you send your Q1 to support@cham.co.uk maybe we can take a quick look to see what your are doing in detail.