Express Introductory Training in ANSYS Fluent Workshop 02 Using the Discrete Phase Model (DPM)

Express Introductory Training in ANSYS Fluent Workshop 02 Using the Discrete Phase Model (DPM) Dimitrios Sofialidis Technical Manager, SimTec Ltd. Mechanical Engineer, PhD PRACE Autumn School 2013 - Industry Oriented HPC Simulations, September 21-27, University of Ljubljana, Faculty of Mechanical Engineering, Ljubljana, Slovenia 2012 ANSYS, Inc. September 19, 2013 1 Release 14.5

Workshop 02 Using the Discrete Phase Model (DPM) 14. 0 Release Introduction to ANSYS Fluent 2012 ANSYS, Inc. September 19, 2013 2 Release 14.5

I Introduction Workshop Description: This workshop shows how to use the Discrete Phase Model (DPM) within Fluent. In the last workshop we simulated the flow of a single phase fluid within a pipe T piece. This workshop will use the same T piece geometry. The DPM enables us to compute the trajectories of a stream of particles/droplets, based on their density and diameter. Learning Aims: This workshop will cover how to set up and run a DPM simulation: Defining particle materials, including turbulent (stochastic) effects, injecting particles into the domain, predicting where erosion will occur. Use either constant or a distribution profile for the particle diameter. Learning Objectives: To understand how Fluent can be used to solve for the flow of a discrete phase, and the key controls used to produce a reliable result. 2012 ANSYS, Inc. September 19, 2013 3 Release 14.5

Simulation to be performed The pipe simulated in workshop 1 is to be fitted in a petrochemicals site. The working fluid will be propane, and upstream some water droplets are injected into the pipe (this is done to dissolve any salts in the gas stream, though that process is not considered here). This simulation will consider how these water droplets are carried by the gas flow, and to what extent they impact on the pipe wall. We will use a range of droplet sizes, and predict where erosion (or in practice, corrosion) may occur on the pipe wall. 2012 ANSYS, Inc. September 19, 2013 4 Release 14.5

Loading a Mesh and Starting Fluent Start a new workbench session. Drag a "FLUENT" component system onto the project. Right click on "Setup", and select "Import Fluent Case", and "Browse...". Browse to and select the file "tpiece_model_from_ws1.cas.gz". Click "OK" on the Fluent Launcherscreen. 2012 ANSYS, Inc. September 19, 2013 5 Release 14.5

Setup of Flow Field We know the mesh is OK (we checked it for Workshop 1). However we need to modify the working fluid to Propane. From the Project schematic (left hand column), select "Materials" then, "Create/Edit...". Click "Fluent Database..." to open a new window. Select "propane (c3h8)", press "Copy", then close both windows. 2012 ANSYS, Inc. September 19, 2013 6 Release 14.5

Assigning Materials Problem "Setup>Materials". Click on "air" then delete This will work, since air is not currently in use. Click on "water liquid" then delete. This will fail, since water is still in use by the cell zone. "Cell Zone Conditions>fluid>Edit". In the pull down list next to Material Name, change to "water" to "propane", then "OK". Revisit the Materials setup, and try again to delete "water liquid". This will now be possible. A common mistake is to merely create the new fluid material, and not assign it to the cell zone. Fluent will still use the default material in the cell zones. Since you cannot delete a material that is in use, this step presents a useful check (especially in complex models). If the unwanted materials are still in use somewhere you cannot delete them. 2012 ANSYS, Inc. September 19, 2013 7 Release 14.5

Obtaining New Flow Field Solution "Methods>Pressure>Standard". All other settings are to remain unchanged from the first workshop. "Solution Initialization>Hybrid Initialization>More Settings>No. of Iterations": "15". "Solution Initialization>Hybrid Initialization>Initialize". "Run Calculation>150 iterations>calculate". The computation takes about 1 minute, and you should see convergence before 150 iterations are reached. 2012 ANSYS, Inc. September 19, 2013 8 Release 14.5

Basic DPM Setup [1] From the project schematic (left hand toolbar), select "Models", "Discrete Phase", then "Edit". On the "Discrete Phase Model" pane, select "Injections". In the "Injections" panel, select "Create". This will open up the "Injections" panel. 2012 ANSYS, Inc. September 19, 2013 9 Release 14.5

Basic DPM Setup [2] Setup a new injection as follows: Set injection type to "surface". Pick surface "inlet z". Keep default material "anthracite". Keep default diameter "uniform". "X Velocity" "0 [m/s]" "Y Velocity" "0 [m/s]" "Z Velocity" " 1 [m/s]" "Diameter" "1e 04 [m]" "Temperature" "90 (c)" "Flow Rate" "1 [kg/s]" Tick "Scale Flow Rate by Face Area". Select "OK" to close this window. "Close" the "Injections" Window. "OK" on the "Discrete Phase Model" window. Only when we have set up a DPM injection can we get access to define the particle material. We will change this on the next slide. There are many ways to introduce DPM particles (parcels). Although here we use a boundary surface present in the geometry, we could choose to inject at XYZ point co ordinates anywhere within the model. 2012 ANSYS, Inc. September 19, 2013 10 Release 14.5

Defining DPM Materials "Materials>Inert Particle>anthracite" and then "Create/Edit". Defining an injection means we can now setup the material properties for the droplets. Change the name from "anthracite" to "water droplets". Change the "Density" to "1000 kg/m^3". Click "Change/Create", then answer "Yes". If we selected "No" then we would have both anthracite and water droplets in the model. Selecting "Yes" overwrites so we just have water droplets present. The injection defined on the last slide will automatically take this new material instead of anthracite. 2012 ANSYS, Inc. September 19, 2013 11 Release 14.5

First Display of Particle Tracks [1] In its simplest form, the DPM can just be used as a post processing exercise (the coupling is one way between the continuous (propane) phase and the droplets). We can go straight to a post processing action. When we display the particle tracks, the solver computes how these particles (of this diameter, density etc) are carried by the flow. "Results>Graphics and Animations>Particle Tracks>Set Up". Select "Draw Mesh", then in the pop up window: Select "Edges", "Edge Type" "Outline". Select all surfaces except "interior fluid". "Display", then close just the "Mesh display" window. If you do not see the pipe outline on screen, then you need to use the pull down panel immediately above the graphic window, and change it from the "Convergence History" plots to "Mesh". 2012 ANSYS, Inc. September 19, 2013 12 Release 14.5

First Display of Particle Tracks [2] On the "Particle Tracks" window, select. "Colour" by "Particle Variables>Particle Diameter". Pick the injection "injection 0". Click "Display". Observe also the bottom line of the TUI window. You should see: Number tracked 142. Number escaped 142. This will be discussed next... 2012 ANSYS, Inc. September 19, 2013 13 Release 14.5

Discussion on DPM [1] In this example, Fluent has released one droplet from each face on the "outlet" boundary. There are 142 faces in the mesh here, hence 142 trajectories. Each droplet has a diameter of 1x10 4 [m], and a density of 1000 [kg/m 3 ]. Therefore each droplet has a mass of 5.2x10 10 [kg] (4/3 rpr 3 ). It is assumed that any droplet released from the same location with the same conditions will follow the same trajectory. Our mass flow rate is 1 [kg/s]. So each of the 142 droplet trajectories computed is used to represent 1.3x10 6 actual [droplets/s] 1/(5.2x10 10 x142). The droplet (or particle) progresses through the domain through a large number of small steps. At each step, the solver computes the force balance acting on a single droplet (diameter 1x10 4 [m]) hence considering the drag with the surrounding fluid, droplet inertia, and if applicable gravity. The mass transported is that of all the droplets in that stream (1.3x10 6 [droplets/s]). 2012 ANSYS, Inc. September 19, 2013 14 Release 14.5

Discussion on DPM [2] The coupling of the droplet (DPM) motion with that of the continuous phase can either be one way or two way coupled. The present example is one way coupled. By this we mean that the fluid affects the momentum/energy of the DPM. But the surrounding fluid flow (propane) remains unaffected by the momentum/energy exchange with the DPM. For this reason, we can use the DPM as a post processing exercise, and quickly compute the particle solution. If required, two way coupled behaviour can be enabled by setting "Interaction with Continuous Phase" on the DPM set up panel. One would then need to perform additional iterations of the (propane) flow field to convergence. It is not usually necessary to solve the DPM at every flow iteration. Typically the DPM field needs updating every 5 10 flow iterations. 2012 ANSYS, Inc. September 19, 2013 15 Release 14.5

Using a Range of Droplet Sizes So far we have looked at droplets of a uniform size. Next we will define a range of diameters. "Define>Injections". Highlight "injection 0" then "Set". Change "Diameter Distribution" to "Rosin Rammler". Set the following values: "Min diameter" "1e 04 [m]". "Max diameter" "5e 04 [m]". "Mean diameter" "4e 04 [m]". All other values should still be the same as set previously. Observe that the default is to have. "Number of Diameters" = "10". Click "OK". 2012 ANSYS, Inc. September 19, 2013 16 Release 14.5

Trajectories of Distributed Sized Droplets On the "Particle Tracks" window, select. "Colour by Particle Variables>Particle Diameter". Pick the injection "injection 0". Click "Display". Observe also the bottom line of the TUI window. You should see: Number tracked 1420. Number escaped 1420. Recall we asked for a distribution of 10 diameters, and so we now have 10 x 142 trajectories being computed. Note how the larger droplet sizes have not made it round the bend, and have impacted on the pipe wall. 2012 ANSYS, Inc. September 19, 2013 17 Release 14.5

Viewing the Range of Sizes Used [1] To plot the size distribution used: "Reports>Discrete Phase>Sample>Set Up". Pick boundary "Outlet", and release from "injection 0", then "Compute". All droplets currently make it to the outlet. This action will write to disk a file called "outlet.dpm" that will record the profile of droplets at this outlet boundary. "Reports>Discrete Phase>Histogram>Set Up". Select "Read" then pick the file just saved ("outlet.dpm"). Select "Sample" "Outlet", "Variable" "diameter" and "Weight" "mass flow". Select "Plot". 2012 ANSYS, Inc. September 19, 2013 18 Release 14.5

Viewing the Range of Sizes Used [2] The Rosin Rammler Diameter distribution is shown in the histogram. Recall the minimum size was 1x10 4 [m] and the maximum 5x10 4 [m]. Since we specified a mean diameter of 4x10 4 [m], the histogram is weighted towards the larger sized droplets. 2012 ANSYS, Inc. September 19, 2013 19 Release 14.5

Trapping Droplets On the Wall By default when DPM droplets/particles hit a wall they are reflected off. In this case we want to say that water droplets that impact on the wall will remain there and not bounce off. "Boundary conditions>wall fluid>edit". On the "DPM" tab, set the "Type" to "trap". Click "OK". 2012 ANSYS, Inc. September 19, 2013 20 Release 14.5

Trajectories With No Reflection On Walls On the "Particle Tracks" window, select. "Colour by Particle Variables>Particle Diameter". Pick the injection "injection 0". Click "Display". Observe also the bottom line of the TUI window. You should see: Number tracked 1420. Number escaped 585. Number trapped 835. Number incomplete 0. It is very important to keep an eye on these numbers. Fluent will simulate a finite number of steps (default 500) for each particle stream. If this is not enough, there may be a significant number "incomplete", in which case the values in Models>Discrete Phase need changing. In some flows the particles may naturally become stuck in a recirculation region, and therefore "incomplete" is appropriate. Now more than 50% of the water droplets impact on the wall and are removed from the simulation. 2012 ANSYS, Inc. September 19, 2013 21 Release 14.5

Including Turbulent Effects This flow is turbulent, which will impart a random motion on the water droplets. However, our flow solution does not resolve all the small scale turbulent eddies in the flow. The way we resolve this is to use stochastic tracking. Put simply, a number (in this case 10) particle streams are released from the same point. Each one is given a random "kick" in each grid cell based on the turbulent intensity. This will indicate how turbulence will modify the trajectories. "Define>Injections". Highlight "injection 0" then "Set". Select "Turbulent Dispersion" tab. Tick "Discrete Random Walk Model". Set "Number of Tries" to "10". "OK". 2012 ANSYS, Inc. September 19, 2013 22 Release 14.5

Trajectories With Turbulent Effects On the "Particle Tracks" window, select. "Colour by Particle Variables>Particle Diameter". Pick the injection "injection 0". Click "Display" This will take noticeably longer than before. Observe also the bottom line of the TUI window. You should see: Number tracked 14200. Number escaped 5719. Number trapped 8481. Number incomplete 0. In this case, the distribution of the number escaped vs the number trapped is barely changed by including turbulent effects. Note that using 10 tries AND 10 particle diameters has resulted in 100x the number of trajectories (142) originally computed. You need to use these settings with care to keep the compute cost manageable. We have just set 10 "tries" for the turbulent tracking, so we now track 10x the number of particle trajectories (previously 1420). 2012 ANSYS, Inc. September 19, 2013 23 Release 14.5

Simulating Erosion [1] We can ask Fluent to account for how the particles interact with the wall, and so simulate erosion. This option is only available if two way coupling has been activated. However we only need to perform 1 iteration to collect this data we are not going to run the model until the two way coupled case converges. First, we will disable turbulent stochastic tracking (for speed reasons) since it was found to have little effect in this case. "Define>Injections". Highlight "injection 0" then "Set". Un Select "Discrete Random Walk". "OK". "Models>Discrete Phase>Edit. Select "Interaction with Continuous Phase". Set "1" to "Number of Continuous Phase Iterations per DPM Iteration". Go to "Physical Models" tab. Enable "Erosion/Accretion" Model. "OK". 2012 ANSYS, Inc. September 19, 2013 24 Release 14.5

Simulating Erosion [2] Run the solver for 1 iteration, so we can compute the erosion quantity. "Solution>Run Calculation>1 iteration>calculate". "Graphics and Animations>Contours>Set Up". Contours of "Discrete Phase Model/DPM Erosion Rate", "Filled" on, "wall fluid". "Display". Rotate the view and look at the Z surface of the pipe, in the region where the droplets hit the pipe wall. The functions used to quantify erosion based on how the DPM parcels impact the wall can be set as part of the wall boundary condition. 2012 ANSYS, Inc. September 19, 2013 25 Release 14.5

Exporting Data to CFD Post Save the project "File>Save As". Fluent saves the values stored in each FLUID grid cell (so propane velocity, temperature pressure etc). BUT the motion of particles is separate. Their trajectories are overlaid on the grid cells, not stored as part of the grid cells. In order to view particle trajectories in CFD Post, these need to be separately exported from Fluent. "File>Export>Particle History Data". Click "Exported Particle Variables". Pick: "Particle Velocity Magnitude", "Diameter" & "Temperature", then "Add Variables", "OK". Select "injection 0" and enter the Particle File Name "t piece dpm". Then "Write". Exit Fluent and return to Workbench. 2012 ANSYS, Inc. September 19, 2013 26 Release 14.5

Preparing for Post From "Component Systems", drag a "Results" object and drop on the FLUENT "Solution" cell. Double click "Results" to launch CFD Post. 2012 ANSYS, Inc. September 19, 2013 27 Release 14.5

CFD Post [1] The results are loaded automatically for the FLUID cells. To load the DPM particle tracks, select. "File>Import>Import Fluent Particle Track File". The file you need is: Folder_where_project_saved\project_name_files\dp0\FLU\Fluent\t piece dpm.xml Select "Open", then "OK". 2012 ANSYS, Inc. September 19, 2013 28 Release 14.5

CFD Post [2] A new item will appear in the model tree "Fluent PT for Water Droplets". This gives access to the data that has been saved per DPM parcel (which is different from the normal results data which is saved per grid cell). Double click on "Fluent PT for Water Droplets". Under "Geometry", set the "Maximum number of Tracks" to "500". Under "Color", set mode to "Variable", and "Variable" "Water Droplets.Particle Diameter". Click "Apply". This will give a similar image to that we saw in Fluent. We exported 1420 particle tracks from Fluent. By plotting 500 tracks we are showing approximately every third particle track. For clarity you may want a number less than 500. 2012 ANSYS, Inc. September 19, 2013 29 Release 14.5

CFD Post [3] Double click on "Fluent PT for Water Droplets". Under "Geometry", set the "Maximum number of Tracks" to "50". Under "Color", set mode to "Variable", and color by "Water Droplets.Particle Time". Under "Symbol", tick "Show Symbols". Set the "Max Time is" to "User Specified" at "0.6 [s]", "Min Time" to "0.0 [s]" and "Interval" to "0.1 [s]". Keep default symbol of "Ball". Click "Apply". The particle tracks are coloured by particle time. The colour legend shows it takes about 0.6s for the water droplets to pass through the model. The symbols are plotted every 0.1s along the trajectories. Initially all the symbols are together in the top pipe, however as they meet the main flow more scatter is evident as some tracks are accelerated more than others. 2012 ANSYS, Inc. September 19, 2013 30 Release 14.5

Wrap Up [1] This workshop has shown how Fluent can be used to simulate the motion of fluid droplets (or solid particles) that are carried along by the fluid. Regular CFD simulations are performed in an "Eulerian" reference frame. The mesh remains fixed, and material flows through the grid (aka mesh) cells. When simulating particle tracks, these move in a "Lagrangian" reference frame. The particles/droplets each have their own X,Y,Z co ordinates and their properties are stored separately from the grid cell (normal data) file quantities. The user sets the diameter and density of the particles to be simulated. The trajectory through the domain is computed over a large number of small steps. At each step their relaxation time can be computed (from knowing their inertia, and the sum of the forces acting on each droplet/particle). Here we have performed several different particle trajectory simulations to investigate: The effect of droplet diameter. The effect of droplets being "trapped" as they hit a wall. The effects of turbulence (random walk model/stochastic tracking). 2012 ANSYS, Inc. September 19, 2013 31 Release 14.5

Wrap Up [2] Using the discrete phase model, there are several other enhancements to this basic setup that we could simulate: Coupling the DPM motion to that of the continuous phase (so that the surrounding propane has its own momentum/temperature modified by the presence of the droplets). Simulating multi component particles: Sample application: An industrial spray drier. Solid particles are introduced which have a moisture content. Thermal energy is taken from the surrounding fluid, the moisture is removed from the particles making them lighter. Simultaneously this water is added in vapour phase to the continuous phase. Simulating reacting particles: Sample application: A coal burner for a power station. The volatile components of the coal particle evaporate, and react with the surrounding air generating heat. 2012 ANSYS, Inc. September 19, 2013 32 Release 14.5