Guidelines for Loss Model setup
|
The Loss model in CFX-5 allows the user to define a pressure drop (as an additional source term in the momentum equations) in a certain region of the domain. This is useful when modelling porous media like catalytic converters, packed beds, membranes, radiator fin packages, and other devices that introduce an additional pressure drop in the fluid but whose geometry is not modelled. Isotropic and directional loss models are available (for isotropic porous regions, or for flow straightening devices such as honeycombs, porous plates, and turning vanes) The source term in the momentum equation is S_i = - (mu/Kperm) * U_i - Kloss * rho/2 * |U|U_i where S_i is a momentum source term, Kperm is the permeability coefficient (for the viscous loss), and Kloss is the resistance loss coefficient (for the inertial loss). The first term represents viscous (linear) losses, whereas the second term represents inertial losses (quadratic). Note that the velocity solved by the code (and assumed by the model) is the superficial fluid velocity. In a porous region, the true fluid velocity of the fluid will be larger because of the flow volume reduction. Sometimes a loss model is formulated in terms of true velocity rather than superficial velocity. If this is the case, the specified coefficients must be adjusted accordingly: the permeability must be multiplied by the porosity, and the loss coefficient must be divided by the porosity squared. The momentum source may also be formulated using linear and quadratic resistance coefficients CR1 and CR2. These coefficients may be related to the permeability and loss coefficients (mentioned above) as follows: CR1 = mu/Kperm CR2 = Kloss * rho/2 When using the Loss model, you will need to set the case appropriately, which basically means: 1) Mesh generation Create a 3D region in the location where loss model is needed. It will be used in CFX-Pre to set the Location of the Subdomain where the Loss model will be setup. Refine the mesh at both sides of all porous media ends, so that flow physics are accurately captured by the solver. Ensure Element Volume Ratios (Volume of one mesh element divided by volume of next element) are less than 1.5 in this region. 2) Set Kperm and Kloss, or CR1 and CR2, to appropriate values. In general, the constant values should come from experimental data spanning the range of velocities for the application. By plotting how the pressure drop changes with the superficial velocity we can determine thevalues of the constants. The equation to plot is: deltaP/Length = CR1 * U - CR2*U^2 If the curve is linear, its slope is CR1. Otherwise the curve must be fitted to a second order polynom (in Excel, Add Trendline), thus allowing to determine both CR1 and CR2. |
||
|