DEM-tutorial

Modeling bubbling fluidized bed using DDPM+DEMIntroductionThe DEM collision model extends the DPM model in Fluent to model dense particulate flows.pneumatic conveying systems, and the flow of slurries. The DEM models is especially useful •When dealing with a wide particle size distribution•When dealing with relatively coarse meshesThis document is a tutorial on the use of the DDPM model where collisions are modeled through DEM model.PrerequisitesThis tutorial will not cover the mechanics of using the Dense DPM or DEM models. It will focus on the application of these models. For more information refer the ANSYS FLUENT User's Guide and Theory Guide. This tutorial is written with the assumption that you have completed Tutorial 1 from the ANSYS FLUENT 14.0 Tutorial Guide, and that you are familiar with the ANSYS FLUENT navigation pane and menu structure. Some steps in the setup and solution procedure will not be shown explicitly.Problem DescriptionIn this tutorial we will model a bubbling fluidized bed and determine its behavior for a given superficial velocity. A rectangular bed of size 0.2m * 0.2m * 0.4m is initially charged with particles, and the superficial velocity of the gas is 0.5 m/s. The pressure drop across the bed is monitored. Schematic of the problem is shown in Figure.1.From the classic fluidization curve, if the superficial velocity of the inlet fluid is small, the bed is not fluidized and behaves like a packed bed. As the velocity of the fluid is increased, the bed begins to fluidize.One of the classical ways to understand the phenomena is the fluidization curve; here the pressure required to pump the fluid at the inlet is studied as a function of the superficial velocity. Under packed bed conditions, there is a linear increase in the pressure as the superficial velocity is increased. However, this increase begins to taper off as the condition of incipient fluidization is reached, and the pressure reaches a constant value (in a time averagedsense). This constant pressure at fluidization conditions is sufficient to maintain the buoyant weight of the bed. In other words<ܲ>௜௡௟௘௧ × ܣ௜௡௟௘௧= Buoyant weight of bedIn this tutorial we will perform simulations for a given superficial velocity where a bed is fluidized. It will be left upon the user to try with different superficial velocity to obtain the fluidization curve.Figure.1: Schematic of problem descriptionPreparationA.Copy the files bed.msh, 92Kparcels.inj and view-0.vw to the working folder.e FLUENT Launcher to start the 3D version of ANSYS FLUENT.Note: For more information about FLUENT Launcher see Section 1.1.2 Starting ANSYS FLUENTusing FLUENT Launcher in the ANSYS FLUENT 14.0 User's Guide.C.Enable DoublePrecision in the Options list.Note: The Display Options are enabled by default. Therefore, after you read in themesh, it will be displayed in the embedded graphics window.Setup and SolutionNote: All entries in setting up this case are in SI units, unless otherwise specified.Step 1: Mesha)Read the mesh file bed.msh.File Read Mesh...Step 2: Generala)Check the mesh.General CheckANSYS FLUENT will perform various checks on the mesh and will report the progress in the console. Ensure that the minimum volume reported is a positive number.b)Enable the transient solver by selecting Transient from the Time list.General TransientStep 3: Modelsa)Multiphase model.Models Multiphase Edit…I.Select Eulerian multiphase model.II.Enable Dense Discrete Phase Model.III.Retain other defaults and click OK.Figure.2: Multiphase Model Panelb)Discrete Phase Model.Models Discrete Phase Edit…I.Make sure that Update DPM Sources Every Flow Iteration.II.Enter 200 for Number of Continuous Phase Iterations per DPM Iteration.III.Make sure that Unsteady Particle Tracking is enabled.IV.Disable Track with Fluid Flow Time Step and enter 0.0002 for Particle Time Step Size (s).V.Enable DEM Collision under Physical Models tab.VI.Set Drag Law as Wen-Yu under Tracking Tab.VII.Set the following under Numerics tab.•Disable Accuracy Control.•Select implicit as Tracking Scheme.VIII.Click OK to close DPM panel.Figure.3: Discrete Phase Model Panelc)Define Injection.Define Injections… CreateI.Select file under Injection Type.II.Select phase-2 under Discrete Phase Domain.III.Enter 1e-8 for Stop Time (s).IV.Click File… button and select 92Kparcels.inj file from working folder.V.Click OK to close Set Injection Properties panel.VI.Click Close to close Injections panel.Figure.4: Set Injection Properties Paneld)Set DEM collision laws.Models Discrete Phase Edit… DEM Collisions…I.Select dem-anthracite and click Set… This will open DEM Collision Settingspanel.II.Select dem-anthracite – dem-aluminum from Collision Pairs.III.Retain spring-dashpot as Normal Contact Force and set friction-dshf for Tangential.IV.Change spring-dashpot: k as 100 and spring-dashpot: eta as 0.5.V.Select dem-anthracite – dem-anthracite from Collision Pairs.VI.Retain spring-dashpot as Normal Contact Force and set friction-dshf for Tangential.VII.Change spring-dashpot: k as 100 and retain other settings.VIII.Click OK to close the panel.IX.Click Close to close DEM Collisions panel.X.Click OK to close DPM panel.Figure.5: DEM Collision Settings PanelStep 4: Phasesa)Set phase-2.Phases Phase-2 Edit...I.Deselect Volume Fraction Approaching Continuous Flow Limit and click OK.Step 5: Operating ConditionsDefine Operating Conditions…a)Enable Gravity and set Z component as -9.81 m/s2.b)Specify Operating Density to be 1.225 kg/m3.Step 6: Boundary ConditionsBoundary Conditionsa)Set boundary conditions for inlet.I.Select inlet from zone list and click Edit… while phase is mixture. This will openVelocity Inlet panel for mixture phase.II.Go to DPM tab and select Discrete Phase BC Type to reflect and DEM Collision Partner as dem-aluminum.III.Click OK to close this panel.IV.Select phase-1 from Phase drop down list and click Edit….V.Enter 0.5 for Velocity Magnitude (m/s) and click OK to close the panel.b)Set boundary conditions for outlet.I.Select outlet from zone list and click Edit…while phase is mixture. This willopen Pressure Outlet panel for mixture phase.II.Go to DPM tab and select Discrete Phase BC Type to reflect and DEM Collision Partner as dem-aluminum.III.Click OK to close this panel.c)Retain default settings for wall.Step 7: Solution MethodsSolution Methodsa)Select Green-Gauss Node Based from Gradient.b)Select QUICK for Momentum and Volume Fraction Spatial Discretization.Step 8: Solution ControlsSolution Controlsa)Set Under-Relaxation Factors for variables as given below.I.Pressure: 0.9II.Momentum: 0.2III.Volume Fraction: 1IV.Discrete Phase Sources: 1Step 9: MonitorsMonitors Surface Monitors Create…a)Create monitor of Area-Weighted Average of Static Pressure on inlet surface.b)Enable Plot and Write.c)Set X Axis as Flow Time and Get Data Every 1 Time Step.d)Click OK to close the panel.Figure.6: Surface Monitor PanelStep 10: Solution InitializationSolution Initializationa)Initialize with default settings. Click Initialize.Step 11: Calculation ActivitiesCalculation Activities Execute Commands Create/Edit…We will define four commands in this step which will save images of particle tracks colored by particle velocity magnitude at specified interval. These images can be clubbed together to create animation.a)Set Defined Commands to 4.b)Set execute commands as shown in the Figure.7 below.c)Set settings for saving images as shown in Figure.8.File Save Picture…Figure.7: Execute Commands PanelFigure.8: Save Picture PanelStep 12: Run CalculationRun CalculationWe will perform this step in three stages. First we will perform calculation for single time step to inject all particles in the domain. We would then set post-processing parameters which would be used to save image files at specific intervals as entered in Step 11. In the second stage, wewould run the calculation for two seconds of flow time with Execute Commands enabled. In the last stage, case will be run for two more seconds without Execute Commands.a)Set Time Step Size (s) as 0.001.b)Set Number of Time Steps as 1.c)Set Reporting Interval as 5.d)Click Calculate.e)Read view-0 from file view-0.vw from working folder.Display Views… Read…f)Create iso-surface of y-coordinate=0. Name it as y=0.Surface Iso-Surface…g)Display contour of phase-2volume fraction on iso-surface y=0. Make sure Filledand Node Values are enabled.Graphics and Animations Contours Set Up…h)Set Light settings. Make sure that Light On and Headlight On are enabled. SelectLighting Method as Gouraud.Display Lights…i)Set particle track settings as shown in Figure.9.Graphics and Animations Particle Tracksj) Click on Attributes… button under Track Style and select Parcel Diameter as shown in Figure.10.k)Click on Filter by… button and select Y-Coordinate and set Filter-Min, Filter-Max as shown in Figure.11.l)Click Display.Figure.9: Particle Tracks PanelFigure.10: Particle Sphere Style Attributes PanelFigure.11: Particle Filter Attributes Panelm)Save the case file as fbed-first-t-step.cas.gz.n)Run calculation for 2000 time steps.o)Disable Execute Commands by setting Defined Commands to 0under Execute Commands panel.p)Run calculation for 2000 time steps.q)Save case and data as fbed-final.cas.gz and fbed-final.dat.gz.Step 13: Resultsa)Figure.12 shows contour plot of secondary phase volume fraction, contour plot ofDPM Concentration and Particle tracks from the final data file. Notice that resultsare close.b)Figure.13shows plot of pressure drop across the bed. Notice that mean value isclose to the pressure drop equivalent for buoyant weight of the bed which is 981 Pa.Figure.12: Results from final data file.A.Contour plot of secondary phase volume fractionB.Contour plot of DPM ConcentrationC.Particle Tracks colored by secondary phase volume fractionFigure.13: Monitor plot for pressure drop across the bed。