Features modeling for CFD

The CFD extension inherits properties from existing features, such as windows, ventilation terminals etc. but some of these needs additional definitions required only for the CFD-model. Here is a list of features that are supported by the CFD extension.

Supply terminal

Air supply terminals from and exhaust terminals to AHUs and fan coils are by default placed in the zone ceiling at the location where arrows are located during animation of air flows. However, the user can specify the position of these terminals by add corresponding objects to a surface.

With the CFD extension installed, the supply terminal form exposes options only used by the CFD extension. These are of two types, named basic and geometric. Each of the types are influenced by the area parameter but in different ways.

Basic supply terminal setting

The basic terminal is simply a circular hole in the wall with the radius defined by the area. During the mesh generation the corresponding patch is generated by selecting a set of faces that fits within the circle, so the exact shape of the patch depend on the mesh resolution. This means that the minimum mesh size much be set small enough to get reasonable resolution of a circle using square faces. A good practice is to have at least 10 cell-width per jet nozzle diameter.

The air flow through this patch is controlled by changing the flow angles which can make the supply terminal patch resemble a diffuser or a jet:

• The Jet creates a homogeneous inflow field at an angle defined by the angle and azimuth parameters. Mind that the resulting flow velocity is the flow-rate divided by the terminal area seen from the angle; A larger angle gives higher velocity for a given flow-rate and area. The angle defines the deviation from the surface normal, whereas the azimuth rotates the resulting flow vector around the surface normal. Thus, if the angle is zero, the azimuth will not have any effect.
• The Diffuser creates a non-homogenous conical and or swirling inflow field. The velocity distribution across the terminal area varies according to the angle, in the same way that the velocity depends on the angle in a jet. An increased cone angle will increase the radial component of the velocity along the radii, whereas increased swirl will increase the tangential velocity (linearly) along the radii. Thus, note that at angles close to 90 degrees, the maximum inflow velocity beomes very large.
  • Example: To model a swirl diffusor that results in a radial flow, attached to the ceiling, set the cone angle to 0 and swirl angle to 65 or 70 degrees.
  • Example: To model a strong diffuser, with very short reach, set swirl angle to 0 and cone angle to 60 degrees.

Geometrically represented supply terminal

An advanced supply terminal consists of a geometrical representation, e.g. a pipe or a rectangular box. Some of the advanced type supply terminals inherit settings from the simple type terminal.

The "Advanced" supply settings selects a geometry to represent the supply. The available geometries are (presently and preferably) very simple. E.g. A rectangular slab, a cylinder, a half cylinder et c. These geometries have in common that they consist of "walls" and one "inflow" surface, which is possible to see in the 3D-view (although the colors are hard to see on some screens, and need to be changed.) The actual velocity depends on all parameters used actually. The geometry size, flowrate, angles, et.c. this is mentioned in the documentation.

Most of these geometries have unit size, so the scaling parameters are used to give them the apropriate dimension: E.g. to create a 160 mm pipe that protrudes 200 mm into the room, scale the cylinder by x=0.16 and y=0.16, z=0.20, then give it a surface offset of 0.20 and view the result in the 3D viewer.

Yes, the radial diffuser have the inflow on the entire mantle area of the cylinder, whereas the end caps are closed.

The pipe-diffusers should be compatible with both Diffuser and Jet settings. The rectangular diffuser only honors the Jet settings.

Exhaust terminal

An exhaust terminal is defined similarly to a supply terminal, but with fewer options. Flow direction and swirl, for instance, has no meaning (no noticable influence) on the flow in the domain.

Fan coils

A fan coil can be simulated/emulated in the CFD simulation by

1. adding a fan coil object to the zone,
2. add a supply and an exhaust terminal, to a zone enclosing element (wall, ceiling or floor), and in each of these select the fan coil as Air source.
3. A geometric, free hanging representation of the device can be achieved by positioning the supply and exhaust close to eachother, and giving them geometrical shapes available from the CFD tab of each terminal.

Thermal beams/Active beams/Baffles

To get a reasonable representation of an active beam in the CFD simulation you must check the Enable CFD representation checkbox.

An active beam can in CFD represented by a flat rectangular geometry with inflow along two (YY) or four (XY) sides and an induced flow (recirculated air) through the base. When the CFD representation is enabled, such a simplified active beam geometry is imported and transformed according to the settings, similar to the supply terminal transformations for geometric supplies.The planeform geometry is given by the shape drawn on the 2D surface (e.g. ceiling) whereas the thickness (default 5 cm) can be scaled using the Scale thickness parameter above.It is advisable to have the 3D-View visible while editing the geometrical parameters of an active beam.

Important

If more than one active beam are connected to one AHU, the entire flowrate is distributed according to the Design airflow setting in the general tab. The respective design air flows are then used as a weighting factor when distributing the air between devices.

If the AHU delivers more air than the sum of all design air flows, all air will still go through the beam(s). No surplus air supply is created. This thus differs from the behaviour of the zone models.

Radiators & Heating/Cooling surfaces

Any radiator or other HC-unit is modeled by a volumetric source term in CFD. The source strength equals the convective heat flux emitted by the unit at the selected instant. The surface (part of the wall, as drawn in the 3D-view or surface-view) behind the radiator is then given an adiabatic boundary condition.

Radiators and other HC-units are not represented in the results table, but can be relied upon to deliver their convective heat directly to the CFD simulation.

Floor heat

Floor heat is treated differently from other HC-units: These are presently modeled by a surface heat flux boundary condition. Again the surface heat flux equals the convective heat flux given by the zone simulation.

Occupants and equipment

Internal gains can be represented either as a volume heat source or as a heat flux from a geometry surface. In the latter case, the gain needs to be associated to an imported geometry or to an extruded geometry by giving the associated gemometry its respective CFD role.

Both occupants and equipment can be associated with imported or extruded geometries, but it is not necessary (actually not even recommended): If an internal gain is not associated to a geometry, it will instead be represented by a local volume heat source. E.g. in the case of an occupant, the convective heat flux calculated by the zone model is added as a source inside a cylinder, that approximately encloses an upright person. In the case of an equipment gain, the cylinder size is related to the area parameter of the equipment object. The location of the heat sources match the location of the gain.

Recommendation

If a zone has a single occupancy internal gain of, say, three persons, position the occupancy on the floor using the floor editor in IDA ICE. Then, to have the occupants added to the CFD simulation, import them as separate geometries, position them at the location of the previously defined occupancy, and then give them the CFD Role "Adiabatic obstruction". This results in a heat source at the approximate location of the "geometric" occupants and also three occupants resolved by CFD simulation (obstructing the flow).