12.1.2. Physics Settings

The Physics Settings tab is present only for combustion simulation.

Combustion Model

Engine Type

If you select Full Engine Full Cycle from the Combustion Simulation Type in the Properties view of ICE cell, then you can select the Engine Type as CI Engine or SI Engine. Else, if you select Sector or Full Engine IVC to EVO the Engine Type selected by default is CI Engine.

Species Model

Depending upon the selection of the Engine Type the choice for Species Model changes.

Depending upon your selection of the Engine Type and Species Model, the tabs activated in the lower half of the Physics Settings tab differ.

Chemistry

In the Chemistry tab you can set the Mixture Properties.

Material Input

For Laminar Finite Rate you can choose Fluent or Chemkin\Thermal Data File from the drop-down list. Else the default selection is Chemkin\Thermal Data File which you cannot modify.

Mixture Material

If you choose Fluent then a few mixture materials that have been chosen from the Fluent materials database will be available to choose from in the Mixture Material drop-down list.

Chemkin File

This allows you to read a chemkin file in which you can provide your own mixture material. This option is available when you choose Chemkin File from the Material Input drop-down list. Click Browse to read the file.

Thermal Data File

This allows you to read a thermodynamic data file. This option is available when you choose Chemkin File from the Material Input drop-down list or when the Species Model is set to Partially Premixed. By default the Thermal Data File from the Fluent installation is chosen. Click Browse to change the file name.

Depending upon the choices you have made for the Mixture Properties, the list in the Initialization tab changes.

Boundary

In this tab you can set the chemical boundary species in consideration. This tab is activated only for the following combinations:

Depending upon your selections in the Chemistry tab the species will be displayed in the Boundary tab. If you have chosen Fluent then the species of the selected Mixture Material will be displayed along with their set Fuel and Oxid values. For a Chemkin file you will have to set the values.

Premix

The Premix tab is activated when you select Partial Premixed from the Species Model drop-down list for SI Engine.

Premixed Model

You can select C Equation or G Equation in the Premixed Model group box.

Flame Speed Model

In the Flame Speed Model group box you can choose the turbulent flame speed model. Depending upon the choice the further options change.

Flame Speed Model

choose from Peters or Zimont from the drop-down list.

Ewald Corrector

is set to Yes by default and described in Peters Flame Speed Model in the Fluent Theory Guide. This option is present only when Peters is selected form the Flame Speed Model drop-down list.

Blind Modifier

is set to No by default. This term is present only for Peters Flame Speed Model.

Flame Curvature

is set to No by default. If it is set to Yes only then the curvature source term in the G-Equation is included. For details check G-Equation Model Theory in Fluent Theory Guide. This term is present only for Peters Flame Speed Model.

Turbulent Length Scale Constant

value is set to 0.37 by default. This term is present only for Zimont Flame Speed Model.

Turbulent Flame Speed Constant

value is set to 0.52 by default. This term is present only for Zimont Flame Speed Model.

Stretch Factor Coefficient

value is set to 0.26 by default. This term is present only for Zimont Flame Speed Model.

Wall Damping Coefficient

value is set to 1 by default.

Turbulent Schmidt Number

value is set to 0.7 by default.

Injection

In the Injection tab you can see that an injection has been setup. Select injection-0 and click Edit to check the injection properties and settings. For more details on the injection settings check the Set Injection Properties dialog box in ANSYS Fluent.

Material

indicates the material for the particles. You can choose from the drop-down menu. If this is the first time you select a particle of this type, you can choose from all of the materials by copying them from the database or creating them from scratch. diesel-liquid is the material chosen by default.

Diameter Distribution

allows you to change from uniform method used to determine the size of the particles in a surface injection, to the rosin-rammler method.

X, Y, and Z Position

indicates the x, y and z position of the injection source/nozzle tip.

X, Y, and Z Axes

indicates the x, y and z components of the vector defining the cone’s axis.

Evaporating Species

(for droplet particles) specifies the gas-phase species created by the vaporization and boiling laws.

Temperature

indicates the initial (absolute) temperature of the injected particle stream.

Start CA

indicates the crank angle at which the injection will start.

End CA

indicates the crank angle at which the injection will stop.

Cone Angle

indicates half of the spray cone angle.

Cone Radius

indicates a non-zero inner radius to model injectors that do not emanate from a single point. The particles will be distributed about the axis with the specified radius.

Total Flow Rate

is the total mass flow rate of all the streams in the group.

Velocity Magnitude

is the velocity magnitude of the particle streams that will be oriented along the specified spray cone.

Min. Diameter

is the smallest diameter to be considered in the size distribution.

Max. Diameter

is the largest diameter to be considered in the size distribution.

Mean Diameter

is the size parameter in the Rosin-Rammler equation.

Spread Parameter

This is the exponential parameter, n, in the Rosin-Rammler equation.

Number of Diameter

indicates the number of diameters in each distribution (that is, the number of different diameters in the stream injected from each face of the surface).

If you have read a profile before then you can select the profile from the drop-down list while setting some of the variables like Cone Angle, Total Flow Rate, and Velocity Magnitude. You can also select PROFILE EDITOR option which will open the Profile Editor dialog box where you can check the plot of the profile or read a new profile.

Default injection is defined based on the geometry information provided in the DesignModeler. For creating additional injections for the simulation use the Create or Copy options. Use Edit to change the properties of the injection.


Note:  If you need to edit multiple injections, you can select them all in the tab and click Edit. This will open up the Injection Properties dialog box which will allow you to edit the properties of all the selected injections at once. Other than the position of the injections all other properties can be edited together.


Flamelet

For the Diesel Unsteady Flamelet species model you will set the flamelet parameters in the Flamelet tab.

Spark

This tab is present only when SI Engine is selected from the Engine Type drop-down list. It allows you to define multiple sparks. Click Create to open the Spark Properties dialog box where you can enter the details required for the spark.

Name

displays the name of the spark being defined.

X, Y, and Z-Center

specifies x, y, and z coordinates of the spark center. These parameters are needed to define the location of the spark.

Initial Radius

specifies the initial spark radius. You can parameterize it by enabling the check box next to it.

Fixed Transition Radius

is set by default to Yes. This will allow you to specify the Transition Radius.

If you select No then ANSYS Fluent will compute the transition radius. For more information see equation 13–1 and 13–2 in Spark Model Theory in the Fluent Theory Guide

Transition Radius

is set to a value here. When the radius reaches this value, ANSYS Fluent automatically switches the spark flame speed model off, so that the flame speed is modeled using the flame speed model that you have selected in the Premix tab. You can parameterize it by enabling the check box next to it.

Start Crank Angle

is the time of spark ignition initialization in crank angle degrees. You can parameterize it by enabling the check box next to it.

Duration

is used to calculate the rate of spark energy input and the time when this input ceases. You can parameterize it by enabling the check box next to it.

Energy

contains the total energy input by the spark. The default energy value is 0. A positive value for energy will cause the temperature of the spark kernel to rise above the combustion process temperature. You can parameterize it by enabling the check box next to it.

Flame Speed Model

allows you to select the turbulent flame speed model for controlling the rate at which the flame front moves.

Turbulent Curvature

includes the effect of flame curvature as specified in Turbulent Curvature in the Fluent Theory Guide.

Turbulent Length

neglects the effects of flame curvature on the flame speed as described in Turbulent Length in the Fluent Theory Guide.

Herweg-Maly

calculates the turbulent flame speed using Herweg-Maly model. See Herweg-Maly in the Fluent Theory Guide.

Laminar

specifies the turbulent flame speed as the laminar flame speed.

Inert

The Inert tab is activated for Partially Premixed and Diesel Unsteady Flamelet Species Model.

In the Inert tab you have three options to choose from the Inert Model drop-down list.

Off

Inert Model is not activated.

Fixed H/C Ratio

Select this option if the hydrogen to carbon ratio is known. For example, for methane (CH4) enter 4 for Fixed H/C Ratio.

Setting the H/C Ratio assumes that the burned gas resulted from the complete, stoichiometric combustion of that hydrocarbon fuel with air, and the only products of the combustion are CO2, H2) and N2.

User Specified

Select this option if you want to specify an arbitrary composition for the inert stream. You can specify the mass fraction for the four species in the default list: CO2, H2O, N2, and O2. Ensure that the sum of the mass fractions add up to 1.

You will need to set appropriate boundary conditions at flow inlets and exits for the inert tracer mass fraction. The tracer species mass fraction must be between zero and one, with the value of one meaning that all of the material entering the domain comes from the inert stream. The values for flow boundaries are set in the Inert Stream field. This is under the Species tab of the inlet or outlet boundary condition dialog box which can be accessed in the Boundary Conditions tab.

You will also need to initialize the Inert Variable in the Initialization tab. For details check Initializing the Inert Stream in Fluent User’s Guide.

You can also patch the inert mass fraction by entering an appropriate value. The Inert Variable is available under the Variable list in the Patching Zones dialog box. For details check Inert Fraction in Fluent User’s Guide.

ANSYS Fluent allows burned gases to be converted to an inert gas. This has been designed with in-cylinder combustion in mind to aid the simulation of multiple cycles of such engines using the partially-premixed combustion model with exhaust gas recirculation (EGR). At the end of a combustion stroke, the premixed progress variable of the burnt gases is unity. When fresh charge, with progress variable of zero, is mixed with the burnt trapped gases, combustion will be initiated unless these trapped gases are converted to inert.

This facility is accessed via the Dynamic Mesh Events. There, you will need to set the crank angle at which the event occurs (usually shortly before the inlet valves open) and at the fluid zones (usually the combustion chamber) where the burnt gases are converted to inert.

In Fluent in Dynamic Mesh Events an Inert EGR Reset event is added. The event is set before IVO. When multiple invalves are present then this event is set for the invalve whose opening crank angle comes first. The Zones set for this event are the chamber zones. For more information go to Resetting Inert EGR in Fluent User’s Guide.

Pollutant

In the Pollutant tab you can use the Nox and Soot Model for modeling Soot formation. Under the Pollutant tab are two tabs: Nox and Soot.

Nox

Nox concentrations generated in combustion systems are generally low. As a result, chemistry has negligible influence on the predicted flow field, temperature, and major combustion product concentrations. It follows that the most efficient way to use the Nox model is as a postprocessor to the main combustion calculation.

Thermal

To enable thermal Nox select Yes from the Thermal drop-down list.

Prompt

To enable prompt Nox select Yes from the Prompt drop-down list.

  • Set the Fuel Carbon Number to specify the number of carbon atoms per fuel molecule.

  • Set the Equivalence Ratio as follows:

    (12–2)

Number of Post Iterations

When either of Thermal or Prompt is enabled then the Number of Post Iterations is set to 10. This will be set in the ANSYS Fluent Run Calculation task page.

Soot

When the mass fraction of soot is relatively large (for example, 10%) the soot formation should be computed as part of the main combustion solution and not through postprocessing.

Soot Model

You can enable and set up the Moss-Brookes soot formation models by selecting Moss-Brookes from the Soot Model drop-down list.

Fuel

Select the fuel from the Fuel drop-down list. If you are using the non-premixed model for the combustion calculation and your fuel stream consists of a mixture of components, you should choose the most appropriate species as the Fuel species for the soot formation model.

Fuel Carbon Number (Soot)

After selecting Fuel species enter the related Fuel Carbon Number for use in the mixture fraction calculation.

Fuel Hydrogen Number

After selecting Fuel species enter the related Fuel Hydrogen Number for use in the mixture fraction calculation.


Note:  When Partially Premixed combustion model is chosen then both Soot and Nox will be PDF mixture. If Chemkin is chosen then both Soot and Nox will be PDF temperature beta 20 with transported variance. These settings are done internally.



Release 18.2 - © ANSYS, Inc. All rights reserved.