Data Loading...
Ansys Fluent_Multiphase_2020R1_WS04.1_Using_DPM Flipbook PDF
Ansys Fluent_Multiphase_2020R1_WS04.1_Using_DPM
117 Views
58 Downloads
FLIP PDF 1.46MB
Ansys Fluent Multiphase Flow Modeling
Using the Discrete Phase Model
Release 2020 R1
© 2020 Ansys, Inc. Unauthorized use, distribution, or duplication is prohibited.
Introduction • This workshop shows how to use the Discrete Phase Model (DPM) within Ansys Fluent. You will first simulate the flow of a single phase fluid within a pipe T-piece, and then use DPM to compute the trajectories. The DPM enables you to compute the trajectories of a stream of particles/droplets through the continuous phase flow, based on their density and diameter. • This workshop will cover how to setup and run a DPM simulation. It will show how to do the following: ‐ Defining particle materials ‐ Injecting particles into the domain ‐ Using either constant or a distribution profile for the particle diameter ‐ Including turbulent (stochastic) effects ‐ Predicting where erosion will occur
2
© 2020 Ansys, Inc. Unauthorized use, distribution, or duplication is prohibited.
Prerequisites This tutorial is written with the assumption that you have completed Tutorial 1 from Ansys Fluent Tutorial Guide, and that you are familiar with the Ansys Fluent tree and ribbon structure. Some steps in the setup and solution procedure will not be shown explicitly.
3
© 2020 Ansys, Inc. Unauthorized use, distribution, or duplication is prohibited.
Problem Description • The flow simulated is in a T-section of a pipeline. The objective is 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. • The pipe used in this simulation is to be fitted in a petrochemicals site. The working fluid will be propane, and some water droplets are injected into the pipe from upstream (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. You will use a range of droplet sizes, and predict where erosion (or in practice, corrosion) may occur on the pipe wall.
4
© 2020 Ansys, Inc. Unauthorized use, distribution, or duplication is prohibited.
Preparation • • • • •
Copy the file tpiece.msh.gz to the working folder. Use the Fluent Launcher to start the 3D version of Ansys Fluent. Enable Double Precision Enable Display Mesh After Reading After Fluent launches, read the mesh File → Read → Mesh... • After the mesh loads, set the temperature units to Celsius • In the Physics tab, activate the energy equation
5
© 2020 Ansys, Inc. Unauthorized use, distribution, or duplication is prohibited.
Materials • Copy Propane from the Materials database. Physics tab → Materials → Create/Edit... ‐ Click Fluent Database... to open the Fluent Database Materials dialog box.
‐ Select propane (c3h8) and click Copy and then Close. ‐ Retain the default property values and close the Create/Edit Materials dialog box.
6
© 2020 Ansys, Inc. Unauthorized use, distribution, or duplication is prohibited.
Cell Zone Conditions • Open the cell zone conditions panel for Fluid and assign the material to be propane
7
© 2020 Ansys, Inc. Unauthorized use, distribution, or duplication is prohibited.
Boundary Conditions Physics tab → Zones group → Boundaries
• Assign the following boundary conditions for inlet-y and inlet-z Boundary
Velocity (m/s)
Temperature (°C)
inlet-y
0.3
15
inlet-z
0.1
25
• outlet and wall-fluid will use default boundary conditions so there is no need to open the panels
8
© 2020 Ansys, Inc. Unauthorized use, distribution, or duplication is prohibited.
Report Definition, Initialize and Solve • In the Solution tab Create a Report Definition for the static pressure at the inlets ‐ ‐ ‐ ‐ ‐ ‐ ‐
Report type = Surface Report > Area Weighted Average… Report Name = "inlet-pressure-report" Field Variable = Static Pressure Surfaces: select both inlet-y and inlet-z Activate the Per Surface option so that each inlet will be plotted in a separate curve Tick the boxes for Report File and Report Plot Click OK
• Click Initialize • Enter 100 iterations and click Calculate ‐ The solution should converge smoothly •
Exact number of iterations may differ from the pictures
• Save the case and data files as tpiece-flow-calc.cas.h5 9
© 2020 Ansys, Inc. Unauthorized use, distribution, or duplication is prohibited.
DPM Injection Setup • Go to the Physics tab, then the Model Specific group, and select Injections under Discrete Phase
• In the Injections panel, click Create (not shown) • Define a surface injection • Release from the inlet-z surface and define properties as below
Click OK when finished 10
© 2020 Ansys, Inc. Unauthorized use, distribution, or duplication is prohibited.
Materials • Open the Materials panel and change the Material Type to inert-particle ‐ The properties of anthracite will be displayed
• Change the name to water-droplets and change the density to 1000 kg/m³ • Click Change/Create at the bottom of the panel ‐ Click Yes when asked if you want to overwrite anthracite ‐ This will cause the injection material to change to water-droplets
11
© 2020 Ansys, Inc. Unauthorized use, distribution, or duplication is prohibited.
Particle Track Display • In the Mesh Display panel, change the options so that only edges which outline the model are displayed • In the Particle Tracks panel, activate Draw Mesh, change the Color by variable to particle diameter and display the particle tracks from injection-0
12
© 2020 Ansys, Inc. Unauthorized use, distribution, or duplication is prohibited.
Discussion
Note: 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).You can go straight to a post-processing action. When you display the particle tracks, the solver computes how these particles (of this diameter, density, etc.) are carried by the flow. 13
© 2020 Ansys, Inc. Unauthorized use, distribution, or duplication is prohibited.
Discussion • You can see the following message in the console: ‐ number tracked = 96, escaped =96
• In this example, Fluent has released one droplet from each face on the inlet-z boundary. There are 96 faces in the mesh here, hence 96 trajectories. ‐ Each droplet has a diameter of 1x10-4 m, and a density of 1000 kg/m3. ‐ Therefore, each droplet has a mass of 5.2x10-10 kg (4/3 ρπr³). ‐ It is assumed that any droplet released from the same location with the same conditions will follow the same trajectory. ‐ Mass flow rate is 1 kg/s. ‐ Therefore, each of the 96 droplet trajectories represents 2.0x107 actual droplets/sec •
1 kg/s ÷ (96 x 5.2x10-10 kg/droplet)
• Each 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) – thus considering the drag with the surrounding fluid, droplet inertia, and gravity if applicable. The mass transported is that of all the droplets in that stream (2.0x107droplets/sec) 14
© 2020 Ansys, Inc. Unauthorized use, distribution, or duplication is prohibited.
Discussion • 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. ‐ This means that the fluid affects the momentum / energy of the DPM. ‐ The surrounding fluid flow (propane) remains unaffected by the momentum / energy exchange with the DPM. ‐ Therefore, you can use the DPM as a post-processing exercise and quickly compute the particle solution.
• If required, two-way coupled behavior can be enabled by setting Interaction with Continuous Phase on the Discrete Phase Model dialog box. ‐ You would then need to perform additional iterations of the (propane) flow field until convergence is reached once again. ‐ It is not usually necessary to solve the DPM at every flow iteration. Typically, the DPM field needs updating only every 5-10 flow iterations.
15
© 2020 Ansys, Inc. Unauthorized use, distribution, or duplication is prohibited.
DPM Injection Modification: Diameter Distribution • Next you will change the particle diameters. Start by opening the Injections panel as shown on Slide 10
• In the Injections panel, select injection-0 and click Set… (not shown) • Change the diameter distribution from Uniform to Rosin-Rammler • Scroll to the bottom of the Point Properties area and enter the following parameters for the distribution ‐ ‐ ‐ ‐
Enter 1e-04 for Min. Diameter (m). Enter 5e-04 for Max. Diameter (m). Enter 4e-04 for Mean Diameter (m). Observe that the Number of Diameters is set to a default value of 10.
• Click OK when finished (not shown)
16
© 2020 Ansys, Inc. Unauthorized use, distribution, or duplication is prohibited.
Particle Track Display • Display the particle tracks again using the previous settings in the Particle Tracks panel ‐ Note how the larger droplet sizes have not made it round the bend and have impacted on the pipe wall.
• You can see the following message in the console: number tracked = 960, escaped =960 ‐ As the value for Number of Diameters is set to 10 on the previous slide, you now have 10 x 96 trajectories being computed
17
© 2020 Ansys, Inc. Unauthorized use, distribution, or duplication is prohibited.
Plot Particle Diameter Distribution (1): Sample Trajectories • In the Results tab, go to Model Specific, select Discrete Phase and then Sample… • In the Sample Trajectories dialog box, select outlet from the list of Boundaries. • Select injection-0 from Release from Injections. • Click Compute and then Close. ‐ This will write a file outlet.dpm to the disk. This file will record the profile of the droplets at the selected boundary, in this case the outlet. All the droplets currently go to the outlet.
18
© 2020 Ansys, Inc. Unauthorized use, distribution, or duplication is prohibited.
Plot Particle Diameter Distribution (2): Histogram (1) • In the Results tab, go to Model Specific, select Discrete Phase and then Histogram… • In the Trajectory Sample Histograms dialog box, click Read... and select the file outlet.dpm. • Select outlet from the Sample list. • Select diameter from the list of Variable.
• Select mass-flow from the list of Weight. • Click Axes… and go to the next slide
19
© 2020 Ansys, Inc. Unauthorized use, distribution, or duplication is prohibited.
Plot Particle Diameter Distribution (2): Histogram (2) • In the Axes – Sample Histogram panel, increase Precision to 5, click Apply and then Close • In the Trajectory Sample Histograms dialog box, click Plot ‐ The Rosin-Rammler Diameter distribution is shown in the histogram. The minimum size set was 1x10-4 m and the maximum 5x10-4 m. Since you have specified a mean diameter of 4x10-4 m, the histogram is weighted towards the larger-sized droplets.
• Close the Trajectory Sample Histograms dialog box
20
© 2020 Ansys, Inc. Unauthorized use, distribution, or duplication is prohibited.
DPM Wall Boundary Condition • Open the boundary conditions panel for wall-fluid and change the DPM boundary condition to trap ‐ Note- By default, DPM droplets/particles are reflected when they hit a wall. This step will change the conditions so that water droplets impacting the wall will remain there and not bounce off.
• Click OK to close the panel • Display the particle tracks using the previous settings ‐ You can see the following message in the console: number tracked = 960, escaped = 630, trapped = 330 ‐ Thus, now 34% of the water droplets impact the wall and are removed from the simulation. 21
© 2020 Ansys, Inc. Unauthorized use, distribution, or duplication is prohibited.
Discussion
Note - It is very important to keep an eye on the values reported for number tracked, escaped, incomplete, and if applicable, other fates. Fluent will simulate a finite number of steps (default 50000 set in the Discrete Phase Model dialog box) for each particle stream. If this is not enough, there may be a significant number of incomplete particles, in which case the values in the Discrete Phase Model dialog box need changing. In some flows, the particles may naturally become stuck in a recirculation region and the presence of incomplete particles is appropriate. 22
© 2020 Ansys, Inc. Unauthorized use, distribution, or duplication is prohibited.
DPM Injection Modification: Turbulent Dispersion • Next you will add turbulent dispersion effects to the particle tracking. Start by opening the Injections panel as shown on Slide 10
• In the Injections panel, select injection-0 and click Set… (not shown) • Click the Turbulent Dispersion tab • Activate Discrete Random Walk Model and increase the Number of Tries to 10 • Click OK when finished (not shown)
23
© 2020 Ansys, Inc. Unauthorized use, distribution, or duplication is prohibited.
Particle Track Display • Display the particle tracks again using the previous settings in the Particle Tracks panel ‐ It will take some time to display. You have just set 10 for Number of Tries for the turbulent tracking, so you now track 10 times the number of particle trajectories (previously 960).
• You can see the following message in the console: number tracked = 9600, escaped = 6073, trapped = 3527 ‐ As the value for Number of Diameters is set to 10 on the previous slide, you now have 10 x 960 trajectories being computed ‐ Using 10 tries and 10 particle diameters, has resulted in 100 times the number of trajectories compared to (96) originally computed. You need to use these settings with care to keep the compute cost manageable. 24
© 2020 Ansys, Inc. Unauthorized use, distribution, or duplication is prohibited.
Erosion • You can check in Fluent how the particles interact with the wall by simulating erosion. This option is only available if two-way coupling has been activated. However, you will need to perform 1 iteration to collect this data. You need not run the model until the two-way coupled case converges. • First, you will disable turbulent stochastic tracking (for speed reasons) since it was found to have little effect in this case. However, for most applications involving erosion modeling, the use of stochastic tracking is required to obtain accurate predictions. ‐ Opening the Injections panel as shown on Slide 10 ‐ Untick Discrete Random Walk Model and then click OK to close the panel
25
© 2020 Ansys, Inc. Unauthorized use, distribution, or duplication is prohibited.
Model Settings for Erosion • In the Physics tab, under the Models group, click Discrete Phase…
• Activate Interaction with Continuous Phase and change the DPM Iteration Interval to 1 • Go to the Physical Models tab and activate Erosion/Accretion • Click OK to close the panel
26
© 2020 Ansys, Inc. Unauthorized use, distribution, or duplication is prohibited.
Calculate Erosion • In the Solution tab, under Run Calculation change the number of iterations to 1 and click Calculate
• Display contours of erosion rate on the wall ‐ Rotate the view and look at the –Z surface of the pipe, in the region where the droplets hit the pipe wall. •
27
Note: 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.
© 2020 Ansys, Inc. Unauthorized use, distribution, or duplication is prohibited.
Summary • 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 mesh cells. When simulating particle tracks, these move in a ‘Lagrangian’ reference frame. The particles/droplets each have their own X,Y,Z coordinates and their properties are stored separately from the grid cell (normal data) file quantities. ‐ You set 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 position and relaxation time can be computed (from knowing their inertia, and the sum of the forces acting on each droplet/particle).
• Here you have performed several different particle-trajectory simulations and studied the following: ‐ 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)
28
© 2020 Ansys, Inc. Unauthorized use, distribution, or duplication is prohibited.
Further Improvements • Using the discrete-phase model, there are several other enhancements to this basic setup that you 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: A sample application is an industrial spray dryer. Solid particles are introduced which have a moisture content. Thermal energy is taken from the surrounding fluid and the moisture is removed from the particles, making them lighter. Simultaneously, this water is added as vapor to the continuous phase. ‐ Simulating reacting particles: A sample application is a coal burner for a power station. The volatile components of the coal particle evaporate and react with the surrounding air, generating heat.
29
© 2020 Ansys, Inc. Unauthorized use, distribution, or duplication is prohibited.
Optional Exercise
Exporting Particle Track Data to CFD-Post
30
Optional: Exporting Particle Data to CFD-Post • Fluent particle track data can be exported to be used in CFD-Post ‐ Fluent saves the values stored in each fluid grid cell (for example, 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.
• Go to File → Export → Particle History Data.. ‐ Select injection-0 from the list of injections
• Click Exported Particle Variables ‐ In the Reporting Variables dialog box, select Particle Velocity Magnitude, Particle Diameter, and Particle Temperature from the Available Particle Variables list. ‐ Click Add Variables. ‐ Click OK to close the Reporting Variables dialog box.
• In the Export Particle History Data panel, change Particle File Name to t-piece-dpm, click Write and then close the panel
31
© 2020 Ansys, Inc. Unauthorized use, distribution, or duplication is prohibited.
Optional: Exporting Particle Data to CFD-Post • Save the case and data files in legacy format ‐ Change the file type as shown before saving ‐ CFD-Post does not support the default .h5 format
• Exit Fluent, launch CFD-Post and load t-piece-flow.dat.gz
• After loading the results, import the particle track file ‐ File → Import → Import FLUENT Particle Track File... ‐ Select the file saved on the previous slide (file extension = .xml) and click OK to close the panel and import the particle tracks ‐ 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).
32
© 2020 Ansys, Inc. Unauthorized use, distribution, or duplication is prohibited.
Optional: Particle Track Display in CFD-Post • Double-click FLUENT PT for Water Droplets in the Outline tree
• In the Details of FLUENT PT for Water Droplets under the Geometry tab, enter 500 for Max Tracks (not shown). • In the Color tab, select Variable from the Mode drop-down list. • Select Water Droplets.Particle Diameter from the Variable drop-down list. • Click Apply.
33
© 2020 Ansys, Inc. Unauthorized use, distribution, or duplication is prohibited.
Optional: CFD-Post Particle Track Display
Note- The image is similar to what you obtained in Fluent. You exported 960 particle tracks from Fluent. By plotting 500 tracks, you are showing approximately every other particle track. For clarity, you may want a number less than 500. 34
© 2020 Ansys, Inc. Unauthorized use, distribution, or duplication is prohibited.
Optional: Modify CFD-Post Particle Track Display • In the Details of FLUENT PT for Water Droplets under the Geometry tab, enter 50 for Max Tracks. (not shown) • In the Color tab, select Water Droplets. Particle Time from the Variable dropdown list. (not shown) • In the Symbol tab, enable Show Symbols. ‐ Retain the selection of User Specified from the Max Time in the drop-down list. ‐ Enter 5.0 [s] for Max Time. ‐ Enter 0.0 [s] for Min Time. ‐ Retain 1.0 [s] for Interval. ‐ Retain the selection of Ball for Symbol. ‐ Click Apply. 35
© 2020 Ansys, Inc. Unauthorized use, distribution, or duplication is prohibited.
Optional: Exit CFD-Post • Save the state file,tpiece-flow-calc.cst. ‐ File → Save State
• Close CFD-Post. ‐ File → Quit
Note -The particle tracks are colored by particle time. The color legend shows it takes about 6.0 s for the water droplets to pass through the model. The symbols are plotted every 1.0 s 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. 36
© 2020 Ansys, Inc. Unauthorized use, distribution, or duplication is prohibited.
End of presentation