Investigation of effect of radial fans scroll housing to the performance of fan with using CFD

Radial fans are using at very wide area such as cooling, ventilation, air-conditioning, dust collecting, drying etc. In tumble dryers, radial fans are important component of the system since radial fan using for circulation of the cycle air. Air, which has heated at the condenser, has high moisture holding capacity. Heated air pass through the high moisture content clothes and clothes get dry because of the cycle air. Radial fan is supply the required airflow. That is why radial fans are essential for drying process. In order to model radial fan with its air channel, Fluent 14.5 CFD code has used which is using finite volume method formulation. Moving reference frame (MRF) method used for modeling interaction between rotor and stator. All of the analysis are calculated for steady state condition. In order to make CFD analysis independent of mesh, mesh independency study has conducted. According to mesh independency work, after 1290000 number of meshes, results are changing about %0,8. Since this value is negligible, all of the CFD works which includes choosing proper turbulence model and parametric work, are conduct with the same mesh configuration. Turbulent flow occurs as a nature of flow inside the radial fans. In order to model turbulent flow, turbulence models are used which are available in Fluent 14.5 CFD code. Three turbulence models are used to validate the model according to the experimental data. These models are Spalart-Allmaras turbulence model, standard k-ε turbulence model and SST k-ω turbulence model, respectively. Spalart-Allmaras model solves only one transport equation for turbulence where other models are solving two transport equations for turbulence. Analyses have done for every turbulence models, which are mentioned above. In order to decide which turbulence model appropriate for the design of casing of radial fan, results for every turbulence model are compared with experimental data. In addition to accuracy, analysis calculation time also consider to choose proper turbulence model. Experiments are performed at wind tunnel, which is prepared for AMCA-207 standard. In addition to wind tunnel tests, two-dimensional PIV measurements performed. Obtained results from PIV showed the velocity vectors and velocity field. PIV results and CFD results showed velocity fields are same for both experimental and numerical. In experimental works, inlet and outlet of air passages are opened to atmosphere. All of the Spalart-Allmaras, standar k-ε and SST k-ω models showed same trend with experimental characteristic curve. However, among all of turbulence models, SST k-ω model showed minimum deviation from characteristic curve which is obtained from experimental work. Instability occured in every turbulence models, when high pressure and low flow rate condition. Not only converging time is increse, but also margin of error increase in case of high pressure and low flow rate. Therefore, in case of high pressure and low flow rate conditions where flow instability increase, using of SMM (Sliding Mesh Method) may increase the accuracy of numerical results. For intermediate range of pressure and flow rate Spalart-Allmaras, standart k-ε and SST k-ω models gave %2,88, %2,95 and %2,03 error respectively. In view of calculation time, analysis with Spalart-Allmaras has minimum time consuming since this model solves only one transport equation for turbulence. Also, analysis with Spalart-Allmaras model is easier to converge than other models. However, other models (standard k-ε and SST k-ω) gave result in five hours. Since, time consuming of other models are not so much, time consuming is not considered for choosing proper turbulence model. SST k-ω turbulence model choosen as a proper turbulence model for the beyond analysis since this model showed not only accurate result but also acceptable time consuming. Rotational motion of rotor, modeled by moving reference frame (MRF, also knwon as frozen rotor) method. In order to obtain characteristic flow rate-pressure curve from CFD calculations, every counter pressure value which is measured at the wind tunnel, given as pressure outlet boundary condition. Also, rotors rotation speed given as boundary condition for every counter pressure value. Inlet of radial fan channel is modeled as opened to the atmosphere and every wall has no-slip condition. From these boundary conditions, radial fans flow rate calculated for every counter pressure value. As a result of series of CFD analysis, characterictic curve of radial fan obtained. As a result of primer numerical calculations, characteristic curves which are obtained from CFD work with Spalart-Allmaras, standard k-ε and SST k-ω turbulence models, have same trend with experimental data. Therefore, acceptable flow rate and pressure data can be calculated from CFD for different radial fan geometries. Margin of error is variable for every counter pressure value. Among the error values, SST k-ω showed less error than other models. In order to find optimal volute geometry, position angle of tongue, diffuser angle after tongue, tongue radius and diameter of suction port parameters are calculated numerically by using CFD. Every parameter choosen as in two different measurements. Also, in every case six different pressure boundary conditions are tested numerically. Therefore, 48 different CFD analysis conducted in order to complete parametric study. Used parameters in the parametric study are chosen from literature survey but their measures are specific according to the dryer chassis. Position angle of tongue is defined as the angle between horizontal axis of rotor and line from the center of tongue to the center of rotor. Tongue radius is defined as radius of curvature of tongue. Diameter of suction port defines diameter of opening in front of rotor suction side. Diffuser angle after tongue parameter defines the angle between wall axis after tongue and vertical axis. Diffuser angle after tongue parameter is not found in the literature survey, this parameter is special for this thesis study. In order to observe, changing of parameters to the radial fan, non dimensional flow and static pressure coefficients are calculted for each CFD results. Since, all of the pressure boundary conditions are the same for every case, pressure coefficients remains same for every parameter. But flow coefficient is always changing with respect to geometry. That is why, variation of flow coefficient is helped to understand the effects of different parameters on the radial fan characteristics. The most effective parameter that effect the flow coefficient is found as diameter of suction port. In case of increase in diameter of suction port, flow coefficient increases %21 with respect to current radial fan and volute geometry. Similarly, in case of decrease in diameter of suction port, flow coefficient decrease %21 with respect to current geometry configuration. Structure of flow at the suction side is observed for suction port parameter. Velocity contours show that, velocity magnitude at the inlet of the suction is almost same for both smaller and larger diameter. Since velocity magnitude is same, flow coefficient is increasing with the larger diameter. Position angle of tongue is found as another effective parameter on the flow coefficient of the radial fan. In case of increase in position angle of tongue, flow coefficient decreases. Especially at the mid range pressure and flow rate zone, flow coefficient decreases %25 with respect to the current geometry if position angle of tongue increases. Similarly, in case of decrease in position angle of tongue, flow coefficient increases about %14 with respect to the current geometry at the mid range pressure and flow rate zone. Radius of tongue and diffuser angle after tongue parameters have negative effect on the flow coefficient. Since these parameters have negative effect, velocity and static pressure fields have not taken into consideration. As a result of parametric CFD analysis, the most effective parameter on the flow coefficient of the radial fan and volute geometry is diameter of suction port. Since velocity magnitude is almost same for smaller and larger suction ports, the one with the larger diameter has larger flow coefficient. The second most effective parameter is position angle of tongue. If position angle of tongue increases, flow rate decreases. Radius of curvature of tongue and diffuser angle after tongue parameters have negative and minor effect on the flow coefficient.