Chapter 20: Selective Catalytic Reduction Simulation

This tutorial is divided into the following sections:

20.1. Introduction

This tutorial illustrates the setup and solution of a Selective Catalytic Reaction (SCR) system calculation using Ansys Fluent. The selective catalytic reduction of nitrogen oxides by injecting reducing agents has received increasing attention in the automotive industry for the removal of harmful gases. Ammonia is typically used as an agent to react with NOx in the presence of catalysts due to the lower exhaust temperature in the diesel engines.

However, to ensure safe and convenient storage and operation, the urea-water solution is often used in automobile after treatment systems. The urea-water solution is injected into the exhaust gas upstream of the SCR catalyst. The liquid jet goes through steps including liquid atomization, evaporation/decomposition and hydrolysis to form a mixture consisting of ammonia, iso-cyanic acid, water vapor, oxygen and other species. The mixture reacts with NOx in the SCR catalyst to reduce the NOx in the exhaust gas stream.

SCR performance is measured on the basis of its de-NOx efficiency, ammonia and iso-cyanic acid slip rates. These parameters heavily depend on the exhaust temperature, the NOx concentration, and the mixture quality at the catalyst inlet, which is mainly determined by the urea injection and decomposition rate.

Mesh file is provided with this tutorial, however the following points need to be considered while creating the geometry and meshing the volume.

Geometric Considerations:

Computational domain consists of three parts:
1. Injector (spray development region).
2. Mixer.
3. Catalyst.
Separate fluid zone needs to be created for catalyst, because it is modelled as porous region.
In place of resolving insulation (mesh inside solid material), it can be modelled using thick-wall (shell-elements) approach.

Note: It is important to model insulation as it influences the wall temperature and hence urea deposition. Resolving the mesh in the insulation region will provide accurate result, but creating mesh in thin walls and insulation can be tedious and CPU intensive. A better approach is available where thermal behavior of insulation and thin metal is modeled with the shell conduction model. This model solves for thermal conduction both in the normal direction, as well as in the planar directions of the wall.

Mesh Considerations:

The following points were considered while meshing the volume:

Spray development region: Uniform mesh.
Boundary layer: 4 inflation layers adjacent to all walls.

This tutorial demonstrates how to do the following:

Use the porous medium model.
Use the laminar finite rate reaction model.
Set up a spray injection of a multicomponent droplet.
Model wall film using SCR specific impingement/splashing model.
Post process results to obtain SCR specific risk analysis evaluation.

20.2. Prerequisites

This tutorial is written with the assumption that you have completed the introductory tutorials found in this manual and that you are familiar with the Ansys Fluent outline view and ribbon structure. Some steps in the setup and solution procedure will not be shown explicitly.

20.3. Problem Description

An automotive selective catalytic reduction system shown in Figure 20.1: Schematic of the selective catalytic reduction system will be modeled.

Figure 20.1: Schematic of the selective catalytic reduction system

In this tutorial you will simulate the injection, liquid atomization, evaporation/decomposition, mixing, and wall film formation and evolution, that takes place inside the automotive SCR systems. To check the performance of the SCR system you will use:

The concept of uniformity index, which gives an indirect indication of the de–NOx efficiency of the SCR system. The area-weighted uniformity index of a specified field variable is defined as:
(20–1)
where is the area–weighted average value and A is the facet area.
SCR specific post–processing tools for assessing the risk for solids deposit formation.

20.4. Setup and Solution

The following sections describe the setup and solution steps for this tutorial:

20.4.1. Preparation

To prepare for running this tutorial:

Download the selective_catalytic_reduction.zip file here .
Unzip selective_catalytic_reactor.zip to your working directory.
The mesh file scr_hexprism.msh.h5 can be found in the folder.
Use the Fluent Launcher to start Ansys Fluent.
Select Solution in the top-left selection list to start Fluent in Solution Mode.
Select 3D under Dimension.
Enable Double Precision under Options.
Set Solver Processes to 4 under Parallel (Local Machine).
Browse to the working directory in General Options tab and press Start button.

20.4.2. Reading and Checking the Mesh

Read the mesh file scr_hexprism.msh.h5.
File → Read → Mesh...
Check the mesh.
Domain → Mesh → Check → Perform Mesh Check
Note: Mesh check will perform various checks and will report the results in the console. Ensure that the reported minimum volume is positive .
The SCR geometric model is a long structure made of various cylindrical co-axial parts of different diameter, joined together by conical transitions. The inlet, outlet and central cylindrical parts have radius of 0.1 [m] and the two larger cylindrical parts have radius of 0.125 [m]; the upstream one contains the mixer, the downstream one the catalyst. The mixer is made of 3 zero–thickness surfaces: wall_mixer–pipes, wall_mixer–plate and wall_mixer–twisted and since they are internal walls, they appear as twins (for example, wall_mixer–pipes and wall_mixer–pipes_shadow).
Note: it’s good practice to display one surface at a time to visually confirm that all surfaces have the intended name. For this tutorial, follow this procedure to familiarize yourself with the model.
Examine the mesh.
Domain → Mesh → Display
1. Select the Edges option and retain the default Faces option in the Options group box.
2. Deselect all surfaces an then select all the wall surfaces by selecting the Wall surface type.
  Click to deselect all surfaces. Click and select Surface Type under Group By to list the surfaces by type, as shown above.
3. Click Display.
4. Rotate and adjust the magnification of the view.
  Figure 20.2: Wall Surface Mesh Display
1. De-select the external wall surfaces wall_ext-catalyst, wall_ext-downstream and wall_ext-upstream.
2. Click Display to show the mixer and close the Mesh Display dialogue box.
  Figure 20.3: Mixer Mesh Display

20.4.3. General Settings

In the Mesh group box of the Domain ribbon tab, set the units for length..

Domain → Mesh → Units...

This opens the Set Units dialog box.

Select length under Quantities.
Select mm under Units.
Select Temperature under Quantities.
Select C under Units.
Close the Set Units dialog box.

20.4.4. Solver Settings

Enable the pressure-based steady solver including the effects of gravity.
Physics → Solver → General
1. Retain the default selection of Pressure-Based from the Type list.
  The pressure-based solver must be used for multiphase calculations.
2. Select Steady from the Time list.
3. Enable Gravity.
4. Enter -9.8065 m/s² for the Gravitational Acceleration in the Y direction.

20.4.5. Specifying the Models

In this tutorial, the energy equation and the species conservation equations will be solved, along with the momentum and continuity equations.

You will use the default settings for the k-ω SST turbulence model, so you can enable it directly from the tree by right-clicking the Viscous node and choosing SST k-omega from the context menu.
Setup → Models → Viscous Model → SST k-omega
Enable chemical species transport and reaction.
Physics → Models → Species...
1. Select Species Transport in the Model list.
2. Enable Volumetric in the Reactions group box.
3. Ensure that Diffusion Energy Source is checked in the Options group box.
4. Select urea–water-air from the Mixture Material drop-down list.
  Note: Assignment of Fluent library mixture material urea–water–air and the activation of volumetric reactions, loads a finite rate chemistry reaction mechanism with two gaseous reactions: CO(NH_2 )_2↔ NH_3+HCNO and HCNO+H_2 O↔ NH_3+CO_2. These species along with air (O2 and N2) are the 7 components of the mixture, shown in Number of Volumetric Species.
5. Click OK to close the Species Model dialog box.
Enable Discrete Phase Model
Physics → Models → Discrete Phase...
1. Enable the Interaction with Continuous Phase in the Interaction group box.
  Note: This is required for the activation of unsteady particle tracking with steady state solver.
2. Set the DPM Iteration Interval to 5.
3. Enable the Unsteady Particle Tracking in the Particle Treatment group box and change the value of Particle Time Step [s] to 0.005.
  Note: Although gas flow can be treated in a steady-state manner, the injection and motion of the droplets must be treated as transient.
4. Increase the Max. Number of Steps in Tracking Parameters group box to 2000.
5. Ensure that the High-Res Tracking is enabled in the Tracking Option group box.
6. Click the Injections button.
  1. Click the Create button.
  2. Select Cone as the Injection Type and set the Number of Streams to 10.
  3. Select Multicomponent as the Particle Type.
  4. Select urea-water from the Material drop-down list.
  5. Select rosin–rammler from the Diameter Distribution drop-down list.
  6. Confirm solid-cone is selected in the Cone Type drop-down list at Cone Injector Parameters group box.
  7. Set the X-Position [m] to 0 mm, Y-Position [mm] to 124 mm, and the Z-Position [mm] to 180 mm.
  8. Set the Temperature [C] to 20 C.
  9. Set the Start Time [s] to 0 s and Stop Time [s] to 1000 s
  10. Set the Azimuthal Start Angle [deg] to 0 degrees and the Azimuthal Stop Angle [deg] to 360 degrees.
  11. Set the X-Axis, Y-Axis and Z-Axis to 0, -0.866 and 0.5, respectively .
  12. Set the Velocity Magnitude [m/s] to 20 m/s.
  13. Set the Cone Angle to 10 degrees.
  14. Set the Outer Radius [mm] to 6.25e-02 mm.
  15. Set the Total Flow Rate [Kg/s] to 5e-05 Kg/s
  16. Set the Min. Diameter [mm] to 4e-03 mm and the Max. Diameter [mm] to 6e-02 mm.
  17. Set the Mean Diameter [mm] to 4e-02 mm.
  18. Set the Spread Parameter to 3.5.
  19. Set the Number of Diameters to 10.
  Note: Start Time and Stop Time are given the above values for the tutorial purposes. For practical SCR applications these should be defined according to the actual urea dosing intervals.
7. In the Turbulent Dispersion tab
8. Select Discrete Random Walk Model.
  Note: This makes sure that particles are not always injected with the same exactly parameters, rather they follow a stochastic behavior with average values as declared in the point properties table above and a perturbation that creates a more realistic turbulence representation.
9. In the Components tab
  1. Select co<nh2>2 for the co<nh2>2<l> Component from the Evaporating Species drop–down list and enter 0.325 for its Mass Fraction.
  2. Select h2o for the <h2o>2<l> Component from the Evaporating Species drop–down list and enter 0.675 for its Mass Fraction.
10. Click OK to close the Set Injection Properties panel.
11. Click Close to close the Injections panel.
12. Click OK to close the Discrete Phase Model panel.
Create another injection by first copying the injection-0.
Setup → Models → Discrete Phase → Injections → Injection-0 Copy...
This will create Injection-1 having the same properties as Injection-0. Change the Value of only the following Variable of Injection-1 in Point Properties tab.
1. Set the X-Position [m] to 4.48 mm, Y-Position [mm] to 123 mm, and the Z-Position [mm] to 172.707 mm.
2. Set the X-Axis to 0.15038.
3. Set the Y-Axis to -0.95511.
4. Set the Z-Axis to 0.25523.
5. Click OK to close the Set Injection Properties panel.
Repeat the procedure to create a third injection by copying injection–1.
Setup → Models → Discrete Phase → Injections → Injection-1 Copy...
This will create Injection-2 having the same properties as Injection-1. Change the Value of only the following Variable of Injection-1 in Point Properties tab.
1. Set the X-Position to -4.48 mm.
2. Set the X-Axis to -0.15038.
3. Click OK to close the Set Injection Properties panel.

20.4.6. Materials

Modify the material properties:

Confirm the properties for the mixture materials.
Setup → Materials → Mixture → urea-water-air Edit...
1. Click the Edit... button to the right of the Mixture Species drop-down list to open the Species dialog box. Confirm that the last of the 7 species on the list Selected Species is n2.
2. Then click Cancel to return to the Create/Edit Materials dialog box.
3. Edit the particle mixture by selecting particle-mixture in the Material Type drop-down list. There is only one item urea-water in theFluent Particle Mixture Materials drop-down list.
4. Select convection/diffusion-controlled for the Vaporization/Boiling Model.
  Note: The convection/diffusion model is recommended for high evaporation rates.
  1. In the Model Options dialog box, enable Variable Lewis Number Formulation in Convection/Diffusion Vaporization Model. This causes the Use the Specific Heat of the Evaporating Species in Boiling Law in Boiling Model to be also enabled.
    Note: Variable Lewis number allows Spalding heat transfer number and Spalding mass number to be different.
  2. Click OK in the Model Options dialog box.
5. Click Change/Create to accept the material property settings.
6. In the Create/Edit Materials dialog box, Select press button Fluent Database… and the dialog box Fluent Database Materials will appear.
  1. Select solid from the Material Type drop-down list and steel from the Fluent Solid Materials list.
  2. Click Copy and close the Fluent Database Materials dialog box.
7. Close the Create/Edit Materials dialog box.

20.4.7. Cell Zone Conditions

Set the cell zone conditions for the catalyst: Setup → Cell Zone Conditions → Fluid → fluid_catalyst Edit...

Enable Porous Zone to activate the porous zone model.
Enable Laminar Zone to solve the flow in the porous zone without turbulence.
Click the Porous Zone tab.
1. Make sure that the principal direction vectors are set as shown in Table 20.1: Values for the Principle Direction Vectors.
  Ansys Fluent automatically calculates the third (Z direction) vector based on your inputs for the first two vectors. The direction vectors determine which axis the viscous and inertial resistance coefficients act upon.
  Table 20.1: Values for the Principle Direction Vectors
  Axis Direction-1 Vector Direction-2 Vector
  X 0 0
  Y 0 1
  Z 1 0
2. For the viscous and inertial resistance directions, enter the values in Table 20.2: Values for the Viscous and Inertial Resistance.
  Scroll down to access the fields that are not initially visible.
  Table 20.2: Values for the Viscous and Inertial Resistance
  Direction Viscous Resistance (1/m²) Inertial Resistance (1/m)
  Direction-1 2e+07 10
  Direction-2 2e+10 10000
  Direction-3 2e+10 10000
  
  Note: This setup provides a finite resistance to flow in the axial Z-direction and practically infinite resistance to the other two directions, therefore straightening the flow along the axial direction. The values of coefficients in Z-direction are estimated from the measured pressure losses along the catalyst, as a function of gases velocity, whereas the coefficients in the other two directions are typically taken to be three orders of magnitude larger.
Click Apply and close the Fluid dialog box.

Axis	Direction-1 Vector	Direction-2 Vector
X	0	0
Y	0	1
Z	1	0

Direction	Viscous Resistance (1/m²)	Inertial Resistance (1/m)
Direction-1	2e+07	10
Direction-2	2e+10	10000
Direction-3	2e+10	10000

20.4.8. Specifying Boundary Conditions

Set the boundary conditions of external wall wall_ext-catalyst.
Setup → Boundary Conditions → Wall → wall_ext-catalyst Edit...
1. Click the Thermal tab.
2. Select Convection under Thermal Conditions and enter 10 for the Heat Transfer Coefficient and -30 for the Free Stream Temperature .
3. Select Steel under Material Name.
4. Enable Shell Conduction and then select Edit.
  1. Enter 1 mm for Thickness.
  2. Select steel from the Material drop down list.
    Note: Shell conduction model allows to use zero–thickness walls, hence saving in mesh count, and simultaneously solve accurately conductive heat transfer inside solids not only along the thickness but also along the wall in both lateral directions, which is necessary in conductive materials such as metals. In case of temperature–dependent solid thermal conductivity and anticipated large variations in temperature, more than one shell layers maybe be necessary to accurately account for the in–thickness temperature distribution.
  3. Click OK in the Conduction Layers dialog box.
5. Select Species tab and confirm that for all species have Specified Mass Flux is selected for the Species Boundary Condition and has a value of 0 specified for the Species Mass Fraction/ Mass Flux.
6. Select the DPM tab.
  1. Select wall-film from the Discrete Phase BC Type drop–down list in the Discrete Phase Model Boundary Conditions group.
  2. Enable Particle–Wall Heat Exchange.
  3. Select stochastic kuhnke from the Impingement/Splashing Model drop-down list in the Impingement/Splashing Parameters group box, retaining the default values.
    Note: Stochastic Kuhnke model is derived from the Kuhnke model and has been developed and calibrated for addressing SCR applications. It introduces stochastic effects into the critical temperature transition process, and the ʺpartial evaporationʺ concept for the evaporative splash regime.
7. Click Apply and close the Wall dialog box.
Set the boundary conditions for internal wall wall_mixer–pipes.
Setup → Boundary Conditions → Wall → wall_mixer–pipes Edit...
1. Click the Thermal tab.
2. Confirm that Coupled is selected in the Thermal Conditions group box.
3. Enable Shell Conduction and then select Edit.
  1. Enter 2 mm for Thickness.
  2. Select steel from the Material drop down list.
  3. Click OK in the Conduction Layers dialog box.
4. Select Species tab and confirm that for all species have Specified Mass Flux is selected for the Species Boundary Condition and has a value of 0 specified for the Species Mass Fraction/ Mass Flux.
5. Select the DPM tab.
  1. Select wall-film from the Discrete Phase BC Type drop–down list in the Discrete Phase Model Boundary Conditions group.
  2. Enable Particle–Wall Heat Exchange.
  3. Select stochastic kuhnke from the Impingement/Splashing Model drop-down list in the Impingement/Splashing Parameters group box, retaining the default values.
6. Click Apply and close the Wall dialog box.
Copy the boundary conditions to the other external walls.
Setup → Boundary Conditions → Wall → wall_ext-catalyst Copy...
1. Ensure that wall_ext–catalyst is selected from the From Boundary Zone list.
2. Select all the walls from the To Boundary Zone list.
3. Click Copy, click OK in the confirmation prompt, and close the Copy Conditions dialog box.
Copy the boundary conditions to the other internal walls.
Setup → Boundary Conditions → Wall → wall_mixer-pipes Copy...
1. Ensure that wall_mixer-pipes is selected from the From Boundary Zone list.
2. Select all the walls from the To Boundary Zone list.
3. Click Copy, click OK in the confirmation prompt, and close the Copy Conditions dialog box.
Set the boundary conditions for the inlet, first change its type from velocity-inlet to mass-flow-inlet.
Setup → Boundary Conditions → Inlet → inlet Type → mass-flow-inlet
Set the conditions for mass-flow-inlet.
1. Enter 0.0347754 kg/s for Mass Flow Rate .
2. Click the Thermal tab and enter 400 C for Total Temperature.
3. Click the Species tab, set the Species Mass Fractions for o2 to 0.001, h2o to 0.08, and co2 to 0.02.
4. Click the DPM tab and confirm that escape is selected for Discrete Phase BC Type.
5. Click Apply and close the Mass Flow Inlet dialog box.
Set the boundary conditions for outlet.
Setup → Boundary Conditions → Outlet → outlet Edit...
1. Click the Thermal tab, enter 400 C for Temperature.
2. Click the Species tab, set all the Backflow Species Mass Fractions to 0.
3. Click the DPM tab and confirm that escape is selected for Discrete Phase BC Type.
4. Click Apply and close the Pressure Oulet dialog box.

20.4.9. Modify the Particle Properties

Thermolysis model applies for both the free particles and wall film. Since wall film is now activated in the boundary conditions thermolysis can now be setup in the materials. Modify the material properties:

Select secondary rate for Thermolysis of particles and wall film:
Setup → Materials → Particle Mixture → urea–water → urea-liquid Edit...
1. Select secondary–rate for the Thermolysis Model.
  Note: Secondary rate thermolysis model allows to define different thermolysis parameters for the particles and film.
  1. Enter 1.0 for the Pre–Exponential Factor in Film Thermolysis Rate group box.
    Click OK to close the Secondary Rate Model dialog box.
Click Change/Create to accept the material property settings.
Close the Create/Edit Materials dialog box.

20.4.10. Flow Simulation

Specify the discretization schemes.
Solution → Solution → Methods...
1. Select SIMPLE from the Pressure-Velocity Coupling drop-down list.
2. Enable Auto Select for the Flux Type.
3. Select Body Force Weighted for Pressure, Second Order Upwind for Momentum, Energy and all the Species in the Spatial Discretization group box.
Set the solution control parameters.
Solution → Solution → Controls...
1. Retain the default Under Relaxation Factors for all variables.
2. Click Limits... to open the Solution Limits dialog box.
  1. Enter -50 C for the Minimum Static Temperature.
  2. Enter 700 C for the Maximum Static Temperature.
  3. Click OK to close the Solution Limits dialog box.
  Note: It's good practice to limit the allowable range of temperature (and/or pressure in other cases) to avoid stability problems.
Create a surface report definition of the species at the interior catalyst.
Solution → Reports → Definitions → New → Surface Report → Uniformity Index-Area Weighted...
1. Enter ui_nh3_cat-in for the Name of the report definition.
2. Enable Report File, Report Plot, and Print to Console in the Create group box.
3. Select Species... and Mass fraction of nh3 from the Field Variable drop-down lists.
4. Select interior_catalyst-in from the Surfaces selection list.
5. Click OK to save the surface report definition and close the Surface Report Definition dialog box.
Create a surface report definition of the velocity at the interior catalyst.
Solution → Reports → Definitions → New → Surface Report → Uniformity Index-Area Weighted...
1. Enter ui_velmag_cat-in for the Name of the report definition.
2. Enable Report File and Report Plot in the Create group box.
3. Select Velocity... and Velocity Magnitude from the Field Variable drop-down lists.
4. Select interior_catalyst-in from the Surfaces selection list.
5. Click OK to save the surface report definition and close the Surface Report Definition dialog box.
Create a surface report definition of the wall film mass.
Solution → Reports → Definitions → New → Surface Report → Sum...
1. Enter sum_wf-mass_walls for the Name of the report definition.
2. Enable separate reporting for each surface by checking Per Surface box in the Options group box.
3. Enable Report File and Report Plot in the Create group box.
4. Select Wall Film... and Wall Film Mass from the Field Variable drop-down lists.
5. Select all the walls from the Surfaces selection list.
6. Click OK to save the surface report definition and close the Surface Report Definition dialog box.
Initialize the flow field using the Initialization group box of the Solution ribbon tab.
Solution → Initialization
1. Retain the default selection of Hybrid from the Method list.
2. Click Initialize.
Save the case and dat file (scr_initial.cas.h5 and scr_initial.dat.h5.)
File → Write → Case & Data...
Request 2000 iterations.
Solution → Run Calculation → Calculate
Note: Convergence in this case is not judged by the residuals, rather from the monitors. Both uniformity monitors show that main phase (gases) flow has been stabilized, whereas the wall film mass monitor suggests, as expected, that disperse phase flow (droplets and wall film) is developing.
1. Figure 20.4: Scaled Residuals
  
  Figure 20.5: Surface Monitor of Uniformity Index (Area–Weighted) for NH3 Mass Fraction at Catalyst Inlet
  
  Figure 20.6: Surface Monitor of Uniformity Index (Area–Weighted) for Mixture Velocity Magnitude at Catalyst Inlet.
  
  Figure 20.7: Surface Monitor of Total Wall Film Mass at Each Wall Boundary.
Save the case and dat file (scr_solved.cas.h5 and scr_solved.dat.h5.)
File → Write → Case & Data...

20.4.11. Postprocessing the Solution Results

Display contours of pressure.
Results → Graphics → Contours → New...
1. Enter pressure_walls for Contour Name.
2. Select Pressure... and Static Pressure from the Contours of drop-down lists.
3. Select Wall from the Surfaces selection list.
4. Click Save/Display.
  Figure 20.8: Static Pressure Distribution on the System Walls.
  
  Contours show that static pressure drops from ~112 to ~2 [Pa] across the catalyst.
5. 1. Disable Global Range and Auto Range in the Options group box.
  2. Change the Min value to 100 [Pa] and the Max value to 120 [Pa].
  3. Click Save/Display.
    Figure 20.9: Static Pressure Distribution on the System Walls; Limited Range.
    
    Contours reveal a smaller pressure drop from ~119 to ~111 [Pa] across the mixer.
Create two longitudinal planes to plot variables at the SCR internal region. These two surfaces will be used to display solution results internally the SCR system.
Create a surface of constant x.
Results → Surface → Create → Iso-Surface...
1. Enter x-mid for New Surface Name.
2. Select Mesh... and X-Coordinate from the Surface of Constant drop-down lists.
3. Click Compute.
  The Min and Max fields display the x-extent of the domain.
4. Retain a value of 0 mm for Iso-Values.
5. Click Create and close the Iso-Surface dialog box.
Repeat steps above and create a surface of constant y.
Results → Surface → Create → Iso-Surface...
1. Enter y-mid for New Surface Name.
2. Select Mesh... and Y-Coordinate from the Surface of Constant drop-down lists.
3. Click Compute.
  The Min and Max fields display the x-extent of the domain.
4. Retain a value of 0 mm for Iso-Values.
5. Click Create and close the Iso-Surface dialog box.
Display the mesh surfaces.
Results → Graphics → Mesh → New...
1. Enter mesh_ext for Mesh Name.
2. Confirm that only Faces have been selected in the Options group box.
3. Select all the Wall surfaces, except those with suffix -shadow. This is to avoid plotting twice the internal (double) walls.
4. Click Save/Display and close the Mesh Display dialog box.
Display contours of gas temperature field inside the SCR with the geometry also displayed.
Results → Graphics → Contours → New...
1. Enter temp_mid-planes for Contour Name.
2. Disable Global Range, Auto Range and Clip to Range in the Options group box.
3. Select Temperature... and Static Temperature from the Contours of drop-down lists.
4. Change the Min value to 300 C.
5. Change the Max value to 400 C.
6. Select Inlet,Outlet and Iso-surface from the Surfaces selection list.
7. Click Save/Display and close the Contours dialog box.
Create a scene containing the static temperature distribution at the two internal surfaces.
Results → Scene New...
1. Change the Name to gas_temp.
2. Change the Title to Mixture Temperature.
3. Enable the mesh_ext and temperature_mid–planes graphics object.
4. Set the Transparency of mesh_ext object to 70.
5. Click Save & Display and close the Scene dialog box.
  Figure 20.10: Static Temperature Distribution at the Two Internal Planes
  
  The gases enter the domain at 400 [C] but when mixed with the cooler droplets (at 20 [C]) and also due to droplets partial evaporation, they are cooled down to an average temperature of ~315 [C] at the outlet. Note that values below the minimum and above the maximum values set in the contour dialog box, are displayed as blue and red, respectively, due to deactivation of Clip to Range option, otherwise they would have been displayed as empty regions.
Create a contour of NH3 distribution on the mixer
Results → Graphics → Contours → New...
1. Enter nh3_int for Contour Name.
2. Disable Global Range in the Options group box.
3. Select Species... and Mass fraction of nh3 from the Contours of drop-down lists.
4. Select all internal walls from the Surfaces selection list.
5. Click Save/Display and close the Contours dialog box.
Figure 20.11: Distribution of NH3 Mass Fraction on the Mixer Walls.
Display contours of Wall Film Height.
Results → Graphics → Contours → New...
1. Enter wfh_ext for Contour Name.
2. Disable Global Range and Auto Range in the Options group box.
3. Select Wall Film... and Wall Film Height from the Contours of drop-down lists.
4. Select the external walls from the Surfaces selection list.
5. Click Compute.
6. Ensure that Clip to Range is selected in the Options group box.
7. Change the Min value to 1e-05 mm.
8. Click Save/Display and close the Contours dialog box.
Create a scene with the wall film height distribution on all walls.
Results → Scene New...
1. Change the Name to wfh.
2. Change the Title to Wall Film Height on External Walls.
3. Enable the mesh_ext and wfh_ext graphics object.
4. Set the Transparency of mesh_ext object to 70.
5. Click Save & Display and close the Scene dialog box.
  Figure 20.12: Distribution of Wall Film Height on the External Walls of the SCR System.
Create a particle tracks graph.
Results → Graphics → Particle Tracks → New...
1. Enter par-tracks_urea for Particle Tracks Name.
2. Select Sphere in the Track Style group box.
3. Click Attributes... and change the Scale to 100.
4. Click Apply and close the Particle Sphere Style Attributes dialogue box.
  This will cause the particles to appear as spheres with a size proportional to their diameter and scaled by x100 for clarity.
5. Select Particle Variables... and Mass Fraction of co<nh2>2<l> from the Color by drop-down lists.
6. Select all three injections from the Release from Injections selection list.
7. Select Summary in the Reporting group box, so that both a summary in the console and a graph in the GUI will be produced.
8. Make sure that both Free Stream Particles and Wall Film Particles are checked.
9. Click Save/Display.
10. Close the Particle Tracks dialog box.
The summary track report provides information about the number of particles in the domain, their fate (ʺevaporatedʺ, ʺtransformedʺ, ʺescapedʺ), their state (ʺIn Filmʺ, ʺIn Fluidʺ) and the associated mass and heat transfer, as well as their composition.
Create a scene with the particle tracks and the walls of the geometry.
Results → Scene New...
1. Change the Name to tracks.
2. Change the Title to Particle Tracks with Urea MF.
3. Enable the mesh_ext and par-tracks_urea graphics object.
4. Set the Transparency of mesh_ext object to 50.
5. Click Save & Display and close the Scene dialog box.
  Figure 20.13: Tracks of Free and Wall Film Particles, Colored by Urea Mass Fraction and Scaled by Particle Diameter.
  
  The particle track graph shows both the cloud of free droplets, as well as the wall particles that form the wall film. It is evident that water content of the droplets is evaporated upstream the mixer and is associated with the cooling effect observed in the gas temperature contour plot previously.
Modify the particles tracks to show only the wall film particles that have lost practically all their water content.
Results → Graphics → Particle Tracks → par-tracks_urea Edit..
1. Uncheck Auto Range to be able to manually set the range of the plotted value.
2. Select Off in the Reporting group box.
3. Uncheck Free Stream Particles to hide them from the display.
4. Set the Min value to 0.999 and the Max value to 1.0, which practically means that all water content of the droplet has evaporated.
5. Check the Filter option.
6. Select Filter By... to regulate filtering.
7. Select Particle Variables... and Mass Fraction of co<nh2>2<l> from the Filter By... drop-down lists.
8. 1. Set the Filter-Min value to 0.999 and Filter-Max value to 1.0 and make sure the remaining settings are as displayed.
  2. Click Apply and close the Particle Filter Attributes dialog box.
9. Click Save/Display and close the Particle Tracks dialog box.
Re-display the scene with the particle tracks and the walls of the geometry.
Results → Scene → tracks Edit...
1. Click Save & Display and close the Scene dialog box.
  Figure 20.14: Tracks of Wall Film Particles with H2O Content Practically Evaporated and Scaled by Particle Diameter.
Save the case and data files (scr_final.cas.h5 and scr_final.dat.h5).
File → Write → Case & Data...

20.5. SCR Specific Post Processing

Ansys Fluent has an automated workflow to post process CFD results and assess the risk for solids deposit formation for SCR systems operating with urea. The calculations involve chemical and hydrodynamic risk factors based on thermodynamic data and known chemical pathways, as well as on experimental evidence reported. The risk variables are defined as dimensionless quantities that vary from 0 (no risk) to 1 (max risk). Note that the risk assessment calculation is not a predictive model for urea deposit formation, and the obtained results should be considered only as rough guidance in exploring urea deposit formation trends. The risk assessment calculation is invoked after initial film formation on SCR surfaces and requires the transient solver.

In the Solver group box of the Physics ribbon tab, select transient.
Physics → Solver → General...
Modify the iterations interval between DPM tracks.
Physics → Models → Discrete Phase...
1. Change the DPM Iteration Interval to 100.
  By setting a value equal or larger than the maximum number of iterations per time step, the particle tracking is only performed once per time step.
2. Click OK to close the Discrete Phase Model panel.
Activate the urea risk assessment from the TUI.
1. Press Enter in the console to get the command prompt (>).
2. Type /define/models/dpm/options/scr-urea-deposition-risk-analysis enable?
3. Type yes in the console and press <Enter>.
4. Type all IDs (provided in the Boundary Conditions list on the model tree) one by one followed by Enter. When the last wall ID has been typed, press Enter again. You should get the following output in the console.
```
/define/models/dpm/options/scr-urea-deposition-risk-analysis> enable
Enable the SCR urea deposition risk analysis? [no] y
Wall face zones(1) [()] 4
Wall face zones(2) [()] 5
Wall face zones(3) [()] 6
Wall face zones(4) [()] 9
Wall face zones(5) [()] 10
Wall face zones(6) [()] 16
Wall face zones(7) [()] 17
Wall face zones(8) [()] 18
Wall face zones(9) [()] 19
Wall face zones(10) [()] 
```
5. Fluent has also activated the Data Sampling for Time Statistics in the Run Calculation Task Page. If Sampling Options... is pressed the details can be seen.
Run the calculation.
Solution → Run Calculation → Run Calculation...
1. Enter 20 for Number of Time Steps. This is a small time period covered, in order to demonstrate the procedure. Larger time periods may be simulated in industrial risk assessment calculations.
2. Ensure that the Time Step Size to 0.005.
3. Enter 10 for Max Iterations/Time Steps. A transient simulation that converges every time step in 10 iterations or less is generally considered to have a sufficiently fine time step size.
4. Click Calculate.
5. Fluent asks if the existing Report files will be over-written or new ones will be created. This happens because now the reports are not monitored every iteration (steady-state solver) but every time step (transient solver). Press Yes to create new files. Fluent starts the transient calculation using the steady-state solution as the initial state of the transient solution. Residuals show that standard convergence is achieved in 10 iterations for all time steps (except a couple of steps at the beginning), which was expected as the steady-state gas flow was quite stable.
Examine the risk levels.
Results → Graphics → Contours → New...
1. Enter risk-analysis for Contour Name.
2. Disable Global Range and Auto Range in the Options group box.
3. Select SCR Urea Deposition Risk Analysis... and SCR Urea Crystallization Risk from the Contours of drop-down lists.
4. Select all walls from the Surfaces selection list.
5. Click Compute. Fluent returns 0 for Min and Max, indicating that risk for crystallization is zero at all walls.
6. Repeat the same for the other two risk parameters, SCR Urea Secondary Reactions Risk and SCR Overall Urea Chemical Deposition Risk, which also return zero risk everywhere.
  Note: Risk assessment for solids deposition in urea SCR systems is based on empirical correlations using parameters reported in the relevant literature. The user can set the values of 9 such parameters through the TUI, according to the specific characteristics of the SCR system simulated.
7. Click Save/Display and close the Contours dialog box.
Modify minimum mass fraction of HNCO from the TUI.
1. Press Enter in the console to get the command prompt (>).
2. Type /define/models/dpm/options/scr-urea-deposition-risk-analysis seco-rx-min-hnco in the console and press Enter.
3. ```
/define/models/dpm/options/scr-urea-deposition-risk-analysis> seco-rx-min-hnco

minimum HNCO mass fraction in the gas phase above the film for secondary reactions [0.03] 0.001
```
4. Type 0.001 in the console and press Enter.
Continue the calculation for another 20 time steps
Re-examine the risk levels.
Results → Graphics → Contours → risk-analysis Edit...
1. Select SCR Urea Deposition Risk Analysis... and SCR Overall Urea Chemical Deposition Risk from the Contours of drop-down lists.
2. Select all walls from the Surfaces selection list.
3. Click Compute and Fluent will return Min and Max values of 0 and 0.5, respectively.
4. Set the Min value to 1e-05.
5. Click Save/Display and close the Contours dialog box.
Create a scene with the overall deposition risk and the walls of the geometry.
Results → Scene New...
1. Change the Name to overall-depo-risk.
2. Change the Title to Overall Deposition Risk.
3. Enable the risk-analysis and mesh_ext graphics object.
4. Set the Transparency of mesh_ext object to 60.
5. Click Save & Display and close the Scene dialog box.
  Figure 20.15: Contours of Overall Deposition Risk on the Walls of the SCR System.
Save the case and data files (scr_transient.cas.h5 and scr_transient.dat.h5).
File → Write → Case & Data...

20.6. Summary

The main focus of this tutorial is to illustrate the setup and solution of a SCR system calculation using Ansys Fluent.