1.5.3. Set Up the Case

Now that the mesh has been defined, you can set up the models and solver options using the guided tasks in the Simulate Workflow tree. In many cases, default parameters are assumed and employed, so that no input is required. The required inputs and changes (non-default) to the setup panels for this case are described here.

Note:  You can change the display properties of items in the 3-D View by selecting them in the Workflow tree and right-clicking then selecting options from the context menu, such as turning ON/OFF their visibility or display of the mesh or level of opacity.

In the Workflow tree, expand Models. In the following steps you will turn ON (check-mark) several models and configure parameters for them in their Editor panels.

  1. Models > Chemistry/Materials: Select Chemistry/Materials. On the Chemistry/Materials icon bar, click the New Import Chemistry   icon. This opens a file browser where you can navigate to a chemistry set file. For this project, however, we use a pre-installed chemistry set that comes with Ansys Forte. This is a simplified, reduced n-heptane mechanism that can be used to represent the diesel fuel under conventional diesel-engine combustion conditions. To load this file, browse to the Data directory and locate the pre-installed file named Diesel_1comp_35sp.cks. The Data directory can be accessed from the file browser by clicking the data radio button in the upper right-hand subpanel of the browser window. The chemistry file is a standard Ansys Chemkin chemistry-set file. (More information about this chemistry set and the files referenced within it can be found in the Appendix E: Fuel Chemistry Sets Included with Ansys Forte in the Ansys Forte User's Guide .)

    Note:  You can respond Yes or No to the "View chemistry set information?" prompt. A Yes response displays the chemistry set file in a viewer.

  2. Models > Transport: For this node, keep all the default settings.

  3. Models > Spray Model: Since this is a direct-injection case, turn ON (check) Spray Model to display its icon (action) bar in the Editor panel.

    1. For the basic Spray Properties, keep the default values: select Radius of Influence Model for the Droplet Collision Model and set 0.2 cm as the Radius of Influence. The Use Vaporization Model option should be ON (checked, its default value).

    2. Create Injector: Click Spray Model in the Workflow tree. The icon bar provides two spray-injector options: Hollow Cone or Solid Cone. For the diesel injector, click the New Solid Cone Injector   icon. In the dialog that opens, name the Solid Cone Injector as "Injector 1". This opens another icon bar and Editor panel for the new solid-cone spray model. In the Editor panel, configure the model parameters for the solid-cone spray model.

      • Composition: Select Create new... in the Composition drop-down menu under Settings and click the Pencil   icon to open the Fuel Mixture Editor. In the Fuel Mixture panel, click the Add Species button and select nc7h16 (that is, n-heptane) as the Species, n-Tetradecane as the Physical Properties and 1.0 as the Mass Fraction. (Note that you must press ENTER after all the values are present in the table.)

      • At the bottom of the panel, type a name for the fuel composition, such as n-heptane. Click Save and Close the window.

      • In the Injector 1 Editor panel, set Inflow Droplet Temperature = 368 K.

      • Under the Injection Type, change the Parcel Specification to Number of Parcels and set Injected Parcel Count = 30,000.

      • Set Spray Initialization to Discharge Coefficient and Angle, and Discharge Coefficient = 0.7, and Cone Angle = 15.0 degrees.

      • Keep default values for Droplet Size Distribution and, under the Solid Cone Breakup Model Settings, the KH Model Constants, RT Model Constants, and Use Gas-Jet Model.

      • Click Apply.

    3. Create a Nozzle: Click the New Nozzle   icon on the Injector 1 icon bar and name the nozzle "Nozzle 1". Nozzle 1 then appears in the Workflow tree, and the Editor panel and icon bar transform to allow specification of the Nozzle geometry and orientation. In the Editor panel, set the Reference Frame parameters to specify the nozzle location and direction. Keep the default Global Origin and use the following settings:

      • Location: Coord. System= Cylindrical, with R = 0.15 cm, Θ = 22.5 degrees, and A = 19.368 cm.

      • Spray Direction: Coord. System= Spherical, with θ = 104.0 degrees, and Φ = 22.5 degrees.

      • Nozzle Size: Area = 0.000302 cm2.

      • Click Apply. You can see the nozzle appear at the top of the geometry. (You may need to make the Geometry non-opaque by right-clicking Geometry and reducing Opacity or changing the color of the nozzle itself, by right-clicking in the Workflow tree on the left side, to make the nozzle easier to see in the interior.)

    4. Create an Injection: In the Workflow tree, click Injector 1 again and click the New Injection   icon on the Injector 1 icon bar and name the injection Injection 1. The new Injection item appears in the Workflow tree, and the Editor panel and the icon bar transform to allow specification of the injection properties. In the Editor panel, select Crank Angle as the Timing option and then expand the subpanel to specify the Start of injection as –22.5 ATDC and Duration of injection as 7.75, respectively. Set the Total Injected Mass = 0.0535 g.

    5. Injection Profile: Click the Create new... option in the profile selection menu next to Velocity Profile, then click the Pencil   icon to open a new window with the Profile Editor. In the Profile Editor window, make sure all the Units are set to None for both columns (the dimensionless data is automatically scaled within Ansys Forte to match the mass and duration of injection) and click the Load CSV button at the bottom of the panel (you may have to expand the panel size to see the button). Navigate to the InjectionProfile.csv file (see Files for the Sample Diesel Sector Case ). Select Comma as the Column delimiter and turn ON Read Column Titles and load the profile file. Alternatively, you can type in the Injection Profile data in the table on the Editor panel or copy and paste from a spreadsheet or 3rd-party editor. Go to Profile Name at the bottom-left of the panel and name the new profile Injection Profile. Once the data is entered, click Save in the Profile Editor and then click Apply in the Editor panel.

      Figure 1.15: Injection Profile Parameter Settings

      Injection Profile Parameter Settings

  4. Models > Soot Model: Turn on the Soot Model. This creates the Settings item. In the Editor panel, do not change any of the defaults.

  5. Boundary Conditions: Under Boundary Conditions in the Workflow tree, specify the boundary conditions in the Editor panels associated with each of the four boundary conditions created by importing the mesh. By default the Wall Model for all of the wall boundaries will be set to Law of the Wall. Leave this default setting as well as the default check box that turns ON heat transfer to the wall.

    • Boundary Conditions > Piston: Set Wall Temperature = 500.0 K. Turn ON Wall Motion with Motion Type set to Slider Crank. The other parameters should be:

    • Stroke = 15.24 cm

    • Connecting Rod Length = 30.48

    • Bore = 13.97 (pre-determined by the Sector Mesh Generator)

    • Accept the defaults of Piston is Offset = unchecked (OFF).

    • For Reference Frame, accept the default Global Origin and Direction parameters.

    • Click Apply.

    • Boundary Conditions > Periodicity: Accept the Sector Angle = 45 degrees, with multi-selected Periodic A and Periodic B boundaries on which to apply this boundary condition.

      Note:  Boundary conditions for sector-mesh cases cannot be modified. They are defined in the file that is imported to start the simulation. Automatic Mesh Generation cases have boundary conditions that can be modified.

    • Boundary Conditions > Head: Set Wall Temperature = 470.0 K. Click Apply.

    • Boundary Conditions > Liner: Set Wall Temperature = 420.0 K. Click Apply.

  6. Initial Conditions > Region 1 Initialization (Main): Specify the parameters for the initial conditions as follows:

    • Composition: Select Constant and then Create new gas mixture... and click the Pencil   icon and to launch the Composition Editor. Set these parameters: set the Composition = Mole Fraction (not the default Mass Fraction). Then click the Add Species button and select both o2 and n2 to add. When both o2 and n2 are in the Species column in the Composition table, enter 0.126 for the o2 Fraction and 0.874 for n2. Name this "Composition 1" in the text field at the bottom of the Gas Mixture window. Click Save.

    • Temperature: Select Constant and then 362.0 K

    • Pressure: Select Constant and then 2.215 bar (Note: this is not the default unit.)

    • Turbulence: Select Constant and then in the pull-down menu for the Turbulence parameters, select Turbulent Kinetic Energy and Length Scale as the way in which we will specify the initial turbulence. For this option we provide an explicit value for the initial turbulent kinetic energy, but use a length-scale approximation to determine the turbulence intensity fraction. Use these values:

    • Turbulent Kinetic Energy = 10,000 cm2/sec2 .

    • Turbulent Length Scale = 1.0 cm

    • Velocity: Select Engine Swirl in the Velocity pull-down and then specify the swirl profile parameters:

      • Initial Swirl Ratio = 0.5

      • Initial Swirl Profile Factor = 3.11

      • Initialize Velocity Components Normal to Piston = ON

      Note:  If you want to estimate the turbulence kinetic energy (TKE) as a fraction of the piston speed, let the fraction be F and stroke is ms-1, the value you would enter then would be

    • Under Piston Boundary, select Piston.

    • Click Apply in the Region 1 Initialization Editor panel.

  7. Simulation Controls: On the Editor panel, under Simulation Limits, for the Simulation End Point Option, specify:

    • Crank Angle Based

    • Initial Crank Angle = -165.0

    • Final Simulation Crank Angle = 125.0 degrees (These two angles correspond to Intake Valve Open and Exhaust Valve Closing, respectively).

    • RPM = 1,200.0

    • Cycle Type is 4-Stroke.

    • Click Apply.

  8. Simulation Controls > Chemistry Solver:

    • Turn ON (check) Use Dynamic Cell Clustering and accept its defaults.

    • Set Activate Chemistry to Conditionally, specifying When Temperature is Reached, setting Threshold Temperature = 600.0 K. Click Apply.

  9. Output Controls > Spatially Resolved: For the Spatially Resolved Output Control, specify:

    • Output Timing Control as Crank Angle.

    • Turn on Interval Based Crank Angle Outputs and set Output every to 5.0 degrees.

    • Also check the box next to User Defined Crank Angle Outputs and then create a table of data using the Profile Editor that contains crank angles going from -22 to +20, with increment 1, units of Angle Degree. Once the profile is saved and named UserCrankAngleOutputs, select it in the User-Defined Crank Angle drop-down menu. This assures that we get more resolved outputs around the spray, without requiring the same resolution throughout the simulation.

    • For Spatially Resolved Species, move these species to the Selection list: nc7h16, o2, n2, co2, h2o, co, no, and no2. Click Apply.

  10. Output Controls > Spatially Averaged And Spray:

    • For the Spatially Averaged Output Control, select the Crank Angle option and specify Output every = 1.0 degree.

    • For Spatially Averaged Species, select all and move all species to the Selection list. Click Apply.

  11. Output Controls > Restart Data: In the Workflow tree, check the box for Restart Data and then in the Restart panel, check the box that says, Write Restart File at Last Simulation Step. Uncheck any other boxes on the panel. Click Apply.

  12. Preview Simulation > Boundary Motion. Accept the defaults and click the Play   icon in the Boundary Motion icon bar. You will see the piston move up and back down the cylinder through the interval defined in the Simulation Limits.

    Note:  If the geometry elements are opaque, the piston is not visible. In this case, go to the Workflow tree on the left-hand side of the Simulate window and right-click Geometry and select Medium as the Opacity. Then make sure the Boundary Condition > Piston visibility   is turned ON.

  13. Save the project at this point using the File > Save command. Then continue to Running Your Quick Start Case [anchor> if you wish to run this case.