Catalyst Tutorial
Catalyst Tutorial |
|
Get necessary files for the Catalyst Tutorial Click on the above hyperlink and copy the all the files to your working directory Major section links are as follows otherwise start from the beginning: STAGE 1 - Tuning the 1D Flow block based on a steady state flow rig analysis
STAGE 2 - Catalyst Flow Distribution Analysis
Prediction of catalyst utilisation using VECTIS VECTIS can be used to predict the flow distribution of a catalyst by modelling either a steady state or transient flow field through the entry channel, entry cone, catalyst brick, exit cone and exit channel. The catalyst brick is represented in the VECTIS CFD calculation using a flow resistance block instead of including the actual brick geometry. This allows the small scale flow effects caused by the brick geometry to be included in the calculation and overcomes the need to model the actual brick geometry which would be too computationally expensive if not impossible. VECTIS has the following options for the flow resistance block
The 1D flow block is most commonly used for catalyst utilisation calculations providing that the model geometry can be rotated such that the axial flow direction is aligned to a co-ordinate axis. If this is not possible the NA1D flow block should be used. This tutorial uses the 1D flow block (option 1 above). The process used to perform the catalyst utilisation calculation is as follows:
STAGE 1 - Tuning the 1D Flow block based on a steady state flow rig analysis The files needed to perform the analysis should be copied to your working directory from the link at the top of this tutorial. This tutorial is not intended to provide information about how to set the complete analysis parameters and instead focuses on the relevant details. Phase1 Geometry and Mesh Setup Detail The FlowBenchSection.tri file is the geometry file that represents the geometry needed to perform the 1D flow block tuning process so that it represents the actual pressure drop of the real catalyst brick. The geometry file should be loaded in to Phase1 and should look as shown below.
The boundaries have been setup to be inlet/outlet surfaces at each end of the channel and a wall surface for the remaining surface. A control mesh named FlowBenchSection.mesh is also provided and should also be loaded into Phase1 and should look as shown below.
The mesh is setup with global cells that are of a similar size to those that will be setup for the actual catalysts analysis in section 2. The cells have dimensions of 8mm in the X and Y directions and also 8mm in the Z direction except for the 1D flow region where the cell length is 9.5mm. This difference in cell length is simply because inside the 1D flow block the flow will be a true axial flow in the Z direction and hence it is possible to have a larger cell spacing. At this stage it should be noted what the cell IJK numbers are that define the 1D flow block volume. To do this turn on the cell numbering in the Option panel and note down the IJK numbers as shown below.
The IJK numbers that will be used to define the 1D flow block volume are:
The computational mesh should now be created. Phase2 and Phase4 Mesh Generation Use the Phase1 > Operations > Generate Mesh panel to enter the name of the mesh as FlowBench and then create the computational mesh as shown below.
The FlowBench.DAT computational mesh file should then be created in the working directory. The INP file for the phase5 solver should now be setup. The FlowBench.INP file is included in the link at the top of this tutorial and should be loaded into Phase5gui. This section will detail the setup parameters that are relevant for the flow bench tuning analysis. The Phase5gui iteration panel is used to choose the Steady State time base and define the start and end iteration number. The post-processing file write frequency is set to the end time since the only results of interest are the final converged results.
The File IO panel is used to define the restart file write frequency to 100 and also to setup 2 monitoring points, one in the inlet side and one in the outlet side. These monitoring points are needed to confirm that each friction factor analysis reaches a converged state.
The Models panel is left a default except for the 1D flow block and the Link file panel. The 1D flow block panel is used to define the IJK number extents that represent the 1D flow volume i.e. the catalyst brick. These IJK numbers were obtained from Phase1. The 1D flow block is setup as a catalyst and the geometric data entered. For the first flow bench analysis the friction factor will be set as 45. This value is obtained either from past experience or from an initial estimation calculation based on the following equation which provides an approximate pressure drop for one catalyst brick channel.
To get the total pressure loss multiply the equation below by the brick cross sectional area *number of cells per unit area. Therefore based on the use of this equation and the fact that the steady state flow rig results show that for a pressure drop of 1000 Pa the mass flow rate is 0.18 Kg/s an estimate for the friction factor can be found. The cross sectional area of the catalyst is 0.01385 m2. The mean axial velocity is therefore 0.18 / (1.201 * 0.01385) = 10.8 m/s. Therefore a first estimate for the friction factor is: 1000 = 0.01385 * 826000 * 0.004 * 0.00001925 * C * 10.8 / (0.001/2) After rearranging this gives a value for the friction factor of: C = 53 Since there will be other losses in the analysis due to the friction and viscous effects the first friction value that will be tried will be a value of 45.
The Models > Time Region panel is also used to define the computational mesh name which is FlowBench.DAT.
The Phase5gui solving panel is used to define a reference pressure position near the outlet. The location of the reference position is not so important since the inlet/outlet boundaries will setup as pressure boundaries so this will fix the absolute pressure. Locating the reference point near the outlet has the advantage that when looking at the relative pressure the pressure is larger near the inlet. The solving panel is also used to define under relaxation factors (URF's) that are slightly smaller than the default values and are as follows:
The URF's are hard set by entering the initial, reference, minimum and maximum to the values in the table above. The Boundary panel is setup to identify the IO boundaries, zero dimensional data set information and the Wall boundary boundary conditions. The steady state flow bench tests are performed by adjusting the mass flow rate to achieve a pressure drop across the catalyst brick of 1000 Pa. The flow bench analyses are therefore setup with a 1.01 bar inlet boundary condition and a 1 bar outlet boundary condition. The zero dimensional data set for the inlet is shown below.
The initial panel is left as default so that phase5gui will use 1bar and 300K as the initial conditions. The first flow bench analysis can now be performed by running phase5. This is done by typing
at a UNIX, LINUX or DOS prompt or by simply using the Phase5gui > File > Run Solver .... option. The calculation should then start and run for 2000 iterations. As the calculation is running the convergence can be monitored by plotting the monitoring point data using RPLOT. An example FlowBench.rp RPLOT file is included with the file for this tutorial and the inlet duct plots are shown below.
It can be seen that the solution has reached a steady converged state after around 600 iterations. The predicted mass flow rate can now be extracted from the results to determine if the chosen friction factor should be reduced or increased. The predicted mass flow rate can either be obtained from the IO files where column 5 is the mass flow rate data or by using the Extract > Flux tool in phase6 and drawing a polygon around an existing mesh plot as shown below.
The analysis should now be repeated with the friction factor set to 25 as shown below.
The mass flow rate for this analysis should then be extracted and the result compared to the measured amount. Now that two flow bench analyses have been performed the friction factor - mass flow rate values can be plotted on a 2D graph as shown below.
A trend line can then be added and the equation of this line used to determine what the friction factor value should be to produce a predicted mass flow rate of 0.18 Kg/s. For this example the required friction factor is: C =(-227.53 * 0.18) + 75.944 = 35 A third flow bench analysis should now be performed with the friction factor set to 35 to confirm that the predicted mass flow rate is approximately equal to 0.18. STAGE 2 - Catalyst Flow Distribution Analysis Now that the 1D flow block setup has been determined the actual catalyst utilisation analysis can be performed. This can be either a transient analysis or a steady state analysis. For this tutorial a steady state analysis will be performed with a constant mass flow rate. Stage 2 Phase1 Geometry and Mesh Setup Detail The Catalyst.tri and Catalyst.mesh files are provided with this tutorial. The Catalyst.tri file should be loaded into Phase1 and the boundary identification should look like that shown below where boundary 1 and 2 are the inlet/outlet boundaries and boundary 3 is the wall surface. This tutorial analysis will involve two catalyst bricks which will be represented by two 1D flow blocks.
The control mesh should also be loaded into phase1. This should look as shown below.
The control mesh has been setup with a global mesh cell size of approximately 8mm except for the cells inside the catalyst bricks which have a cell size of 9.5mm in the axial flow direction. 3 IJK refinement blocks have also been included with refinement levels of 1 1 so that the cells in the entry and exit cones and the volume between the bricks are subdivided to create a cell size of 4mm. This is to provide more accuracy in the critical regions. Stage 2 Phase2 and Phase4 Mesh Generation The computational mesh should now be created by either using the Phase1 > Operations > Generate Mesh panel and defining a name of Catalyst for the output file or by typing:
followed by:
at a DOS, UNIX or LINUX command prompt. The Catalyst.DAT computational mesh file should now be have been created and could be loaded into Phase1 if required. Stage 2 Phase5gui - solver setup The Catalyst.INP file is provided with this tutorial and only the relevant sections of Phase5gui will be detailed here. The Iteration panel is used to select the steady state solver and define the end iteration number and Postprocessing file write frequency equal to 1500. This is typical for a steady state analysis. The convergence can be monitored as the calculation is being performed so that if the convergence is achieved before this number of iterations the solver can be stopped and a POST file created.
The File IO panel is used to define the restart file write frequency equal to 100 and to also setup 5 monitoring points located in the entry duct, entry cone, volume between the bricks, exit cone and exit duct. This number of monitoring points should ensure that the convergence can be monitored at all critical locations so that a definite decision about the status of the calculation can be made.
The Models panel is left as default except that the 1D flow block panel is used to define the location and parameters of the 1D flow regions used to represent the catalyst bricks. Also the Time Region setup panel is used to define the computational mesh name as Catalyst.DAT.
Two 1D flow blocks are setup to represent the two catalyst bricks. The IJK locations are entered to define the volume that should be inside the 1D flow blocks. These cell numbers can be obtained from Phase1 by turning on the Number Cells option whilst the Catalyst.tri and Catalyst.mesh file is loaded. Also the geometric data and friction factor should be defined. This should be exactly the same as that used in the final flow bench analysis i.e. the tuned 1D flow block setup. The Solving panel is used to turn on the required equations and the Boundary panel is used to define a mass flow inlet boundary with 0.18 Kg/s flow rate and a static pressure outlet boundary of 1 bar. The wall set as a constant 300 Kelvin's temperature boundary. The Initial panel is used to define an initial condition flow field of 1 bar and 300K. Step 2 Phase5 - running the analysis Now that the computational mesh and the solver input file have been created the phase5 solver can be started. This is done by either using the Phase5gui > File > Run Solver ... option or by typing the following command at a DOS, UNIX or LINUX command prompt.
The calculation should then start and information about the solution printed to the screen. As the solver is running the data from the monitoring points as well as the residual values can be used to determine when the solution has converged. The Catalysts.rp RPLOT file is provided with this tutorial and can be used for this. After 1500 iterations the plots should look similar to the one shown below.
It can be seen that the analysis is converged after around 800 iterations after viewing all the monitoring point data. Therefore the analysis could be stopped at around 800 iterations using RUN_CONTROL and a POST file created or it can be left to continue to the defined end time of 1500 iterations. Stage 2 Phase6 - Postprocessing When the phase5 solver has finished a POST file should be created that can then be loaded into Phase6. A J=7 scalar plane can be added to confirm the result as well as velocity vector plots etc.
The utilisation information for the catalyst bricks can now be extracted by firstly adding a scalar plane just inside the catalyst bricks which is the K=27 and K=43 planes, selecting the displayed scalar to be the velocity magnitude and then using the Plot > Information tool to calculate the mal-distribution and also the uniformity index. If the analysis was a transient analysis the Time Control > Time Average tool could be used to average the results before extracting the uniformity data.
The Mal-distribution Index is a number between 0 and 1 where 0 is a perfect distribution. It can be described by looking at the figure below.
For an ideal catalyst when plotting the % flow flow area against the percent of flow passing through that area the relationship would be linear so that 50% or the area is be utilised by 50% of the flow for example. This ideal relationship is shown by area B above. In reality this is not the situation and the relationship is typically as that shown by the region A above. So the mal-distribution index is the ration of area A divided by B and hence the lower the mal-distribution value the better the catalyst utilisation. The uniformity index is a statistical measure of the catalyst utilisation which is between 0 and 1. However with the uniformity index a value of 1 indicates a perfect brick utilisation. The equation used to calculate the uniformity index is shown below.
Typical engineering ranges for the uniformity index would be from 0.7 to 0.99 where a value above 0.9 would be considered to indicate a good brick utilisation.
|
