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
model is as a postprocessor
to the main combustion calculation.
The recommended procedure is as follows:
Calculate your combustion problem using ANSYS Fluent as usual.
Important: The premixed combustion model is not compatible with the model.
Important: If you plan to use the ANSYS Fluent SNCR model for reduction,
you must first include ammonia or urea (depending upon which reagent
is employed) as a fluid species in the main combustion calculation
and define appropriate ammonia injections, as described later in this
section. See Defining the Species in the Mixture for details
about adding species to your model and Setting Initial Conditions for the Discrete Phase for details about creating
injections.
Enable the desired models (thermal,
prompt, fuel, and/or
intermediate
, with or without
reburn), define the fuel streams (for prompt
and fuel
only),
and set the appropriate parameters, as described in this section.
Setup → Models → Species → NOx
Edit...
Define the boundary conditions for (and
,
, or
, if necessary)
at flow inlets.
Setup →
Boundary Conditions
In the Equations Dialog Box, turn off
the solution of all variables except species (and
,
, or
, based on
the model selected).
Solution →
Controls
→ Equations...
Perform calculations until convergence (that is, until
the —and
,
, or
, if solved—species
residuals are below
) to ensure
that the
and
or
concentration
fields are no longer evolving.
Solution →
Run Calculation
Review the mass fractions of (and
,
, or
) by generating
graphical plots or alphanumeric reports in the usual way.
Save a new set of case and data files, if desired.
File → Write → Case & Data...
Inputs specific to the calculation of formation
are explained in the remainder of this section.
To enable the models and set related parameters,
you will use the NOx Model Dialog Box (for example, Figure 21.1: The NOx Model Dialog Box).
Setup → Models → Species → NOx
Edit...
In the Formation tab, select the models
under Pathways to be used in the calculation
of the
and
,
, or
concentrations:
To enable thermal , turn on the Thermal NOx option.
To enable prompt , turn on the Prompt
NOx option.
To enable fuel , turn on the Fuel
NOx option.
Important: When using the non-premixed combustion model, the following limitation exist for the Fuel NOx option:
The Fuel NOx option is only available if the DPM model is also enabled.
To enable the formation of through an
intermediate,
turn on the N2O Intermediate option. (Note that
the N2O Intermediate option will not appear until
you have enabled one of the other
models listed
above.)
Your selection(s) under Pathways will enable
the calculation of thermal, prompt, fuel, and/or -intermediate
in
accordance with the chemical kinetic models described in Thermal NOx Formation through NOx Formation from Intermediate N2O in the Theory Guide. Mean
formation
rates will be computed directly from mean concentrations and temperature
in the flow field.
When modeling fuel formation, ANSYS Fluent allows
you to define up to three separate fuel streams, and to select the
fuel
sources for each fuel stream.
You can define multiple fuel streams to include in your model with the following configurations:
Solid and liquid fuels (combusting particle and droplet)
both contributing to fuel .
Two or three solid fuels with different -content
and
model parameters (two or three
combusting particles), for example coal blends, coal-biomass cofiring,
and so on.
Two or three liquid fuels with different -content
and
model parameters (two or three
droplet or multicomponent particles).
Gas and solid (or droplet) fuel both contributing
to fuel .
In addition,
you can model one solid fuel contributing to in the presence
of another reacting solid particle not containing any
, for
example sorbent injection in a coal furnace, calcination reaction
in cement kiln and so on, by specifying the active
fuel
source for
formation. For this configuration,
you will not need to define multiple fuel streams in your model.
If Fuel NOx is enabled in the Pathways group box in the Formation tab, perform the following steps to define multiple fuel streams:
Specify the Number of Fuel Streams in the Fuel Streams group box.
Note: You are allowed up to three separate fuel streams.
Define the first fuel stream.
Select the fuel stream to be defined by using the arrow keys of the Fuel Stream ID field.
Select the Fuel Type in the Fuel tab for the Formation Model Parameters.
If your Fuel Type is Liquid or Solid, select the N sources from the Fuel Sources list.
If the Fuel Type is Solid and you have defined multiple injections with different
combusting particle materials in your reacting flow calculation, the
available combusting particle materials will be listed in the Fuel Sources list. Select one or more materials from the
list to be included as fuel sources in the Fuel NOx calculation. Your selection will be used to determine the char burnout
rate and volatile
release rate
in the coal fuel
formation
rate models described in Fuel NOx from Coal in the Theory Guide. Make sure to deselect all
combusting particle materials that do not contribute to
.
If the Fuel Type is Liquid and you have defined multiple injections with different
droplet or multicomponent particle materials in your reacting flow
calculation, the available materials will be listed in the Fuel Sources list. Select one or more materials from the
list to be included as fuel sources in the Fuel NOx calculation. Your selection will be used to determine the fuel release
rate in the liquid fuel
formation
rate models described in Fuel NOx from Intermediate Hydrogen Cyanide (HCN) and Fuel NOx from Intermediate Ammonia (NH3) in the Theory Guide. Make sure
to deselect all droplet and multicomponent materials that do not contribute
to
.
If you are also modeling Prompt NOx, select the fuel species from the Fuel Species list. You cannot select more than 5 fuel species for each fuel stream, and the total number of fuel species selected for all the fuel streams combined cannot exceed 10. You can define the same, or different Fuel Species, Fuel Carbon Number and Equivalence Ratio for each stream. The Fuel Carbon Number and Equivalence Ratio can be modified in the Prompt tab under Formation Model Parameters.
If the Fuel Type in your model
is Gas, select one or more materials from the Fuel Species list. Your selection will be used to determine
the mean limiting reaction rate in the gaseous fuel
formation
rate models described in Fuel NOx from Intermediate Hydrogen Cyanide (HCN) and Fuel NOx from Intermediate Ammonia (NH3) in the Theory Guide. If you
are also modeling Prompt NOx formation, the same
fuel selection will apply also for the prompt
model.
Set the other parameters associated with your selected pathway(s) in the Prompt and/or Fuel tabs under Formation Model Parameters. See Setting Prompt NOx Parameters and Setting Fuel NOx Parameters for details.
Repeat steps 2.(a)–2.(f) for each additional fuel stream.
Important: The gaseous fuel option is available only when the species model is enabled.
Important: Important considerations should be made when reading case and data files set up in a version of ANSYS Fluent 14.5 or earlier:
When reading a case and data file with multiple injection
materials that was set up in a version of ANSYS Fluent previous to and
including 14.5, ANSYS Fluent will initialize the injection material specific
fuel N sources for the fuel model. ANSYS Fluent will perform
a DPM iteration when the flow iterations are initiated.
When reading a case file that was set up in a version older than ANSYS Fluent 14.5 with multiple fuel streams defined for the Fuel NOx model, you must review the setup and select the N sources from the Fuel Sources list.
You can choose to specify a user-defined function for the rate
of production. By default, the
rate returned from the UDF is added to the rate returned from the
standard
production options, if any
are selected. You also have the option of replacing any or all of ANSYS Fluent’s
rate
calculations with your own user-defined
rate.
In addition to or instead of using the UDF to specify the rate,
you can use it to specify custom values for the maximum limit (
) that is used for the integration of the temperature
PDF (when temperature is accounted for in the turbulence interaction
modeling).
To use a UDF to add a rate to ANSYS Fluent’s rate
calculations, you must compile and load the desired function, and
then select it from the NOx Rate drop-down list
in the User-Defined Functions group box in the Formation tab. After you have selected the UDF, you have
the following options:
You can specify that your custom rate is added to
the ANSYS Fluent rate calculations, by
retaining the default selection of Add to Fluent Rate in the UDF Rate group box for the appropriate
formation
pathway(s) (for example, in the Fuel tab).
You can replace the ANSYS Fluent rate
calculations with your custom rate, by selecting Replace Fluent Rate in the UDF Rate group box for the appropriate
formation
pathway(s) (for example, in the Fuel tab).
You can specify custom values for , by selecting user-defined from
the Tmax Option drop-down list in the Turbulence Interaction Mode tab.
See the Fluent Customization Manual for details about user-defined functions.
The routines employ three methods
for calculation of thermal
(as described in Method 1: Equilibrium Approach in the Theory Guide). You will
specify the method to be used in the Thermal tab,
under Formation Model Parameters in the NOx Model Dialog Box:
To choose the equilibrium method, select equilibrium in the [O] Model drop-down list.
To choose the partial equilibrium method, select partial-equilibrium in the [O] Model or [OH] Model drop-down list.
To use the predicted and/or
concentration,
select instantaneous in the [O] Model or [OH] Model drop-down list.
Important: Note that the urea model uses the [] model.
If you hooked a user-defined function in the Formation tab, you can make a selection in the UDF Rate group box to specify the treatment of the user-defined rate:
Select Replace Fluent Rate to
replace ANSYS Fluent’s thermal rate calculations
with the custom
rate produced by your UDF.
Select Add to Fluent Rate to
add the custom rate produced by your UDF to ANSYS Fluent’s
thermal
rate calculations.
Prompt formation is predicted
using Equation 14–26 and Equation 14–28 in the Theory Guide. For each fuel stream specified in the Fuel Stream ID field in the Formation tab, set the parameters
in the Prompt tab under Formation Model
Parameters in the NOx Model Dialog Box in
the following manner:
If you hooked a user-defined function in the Formation tab, you can make a selection in the UDF Rate group box to specify the treatment of the user-defined rate:
Select Replace Fluent Rate to
replace ANSYS Fluent’s prompt rate calculations with the
custom
rate produced by your UDF.
Select Add to Fluent Rate to
add the custom rate produced by your UDF to ANSYS Fluent’s
prompt
rate calculations.
When using the fuel model, you must set the parameters
in the Fuel tab under Formation Model
Parameters for each fuel stream specified in the Fuel Stream ID field in the Formation tab.
If you hooked a user-defined function in the Formation tab, you can make a selection in the UDF Rate group box to specify the treatment of the user-defined rate:
Select Replace Fluent Rate to
replace ANSYS Fluent’s fuel rate calculations with the
custom
rate produced by your UDF.
Select Add to Fluent Rate to
add the custom rate produced by your UDF to ANSYS Fluent’s
fuel
rate calculations.
If there is no rate UDF or if you selected Add to Fluent Rate, you must define fuel parameters.
To begin, specify the fuel type in the following manner:
For solid fuel , select Solid under Fuel Type.
For liquid fuel , select Liquid under Fuel Type.
For gaseous fuel , select Gas under Fuel Type.
Note that you can use only one of the fuel types for a given fuel stream. The Gas option is available only when the Species Transport model is enabled (see Enabling Species Transport and Reactions and Choosing the Mixture Material).
If you have selected Gas or Liquid as the Fuel Type, you must also specify the following:
Select the intermediate species (hcn, nh3, or hcn/nh3/no) in the N Intermediate drop-down list.
Set the correct mass fraction of nitrogen in the fuel (kg nitrogen per kg fuel) in the Fuel N Mass Fraction field.
Specify the overall fraction of the fuel , by mass, that will
be converted to the intermediate species and/or product
in
the Conversion Fraction field. The Conversion Fraction for the N Intermediate has a default value of 1. Therefore, any remaining
will not contribute
to
formation. This is based
on the assumption that the remaining volatile
will convert to gas phase nitrogen.
However, this has very little effect on the overall mass fraction
of gas phase nitrogen. Therefore, you do not have to solve for nitrogen
species when solving pollutant transport equations.
If you selected hcn/nh3/no as
the intermediate, specify the fraction of the converted fuel , by mass, that will
become hcn and nh3 under Partition Fractions. The fraction of fuel
that will become
will
be calculated by the remainder.
Note that setting a partition
fraction of 0 for both and
is equivalent to assuming
that all fuel
is converted to the final product
,
whereas a partition fraction of 0 for
and 1 for
is the same
as selecting nh3 as the intermediate.
ANSYS Fluent will use Equation 14–31 and Equation 14–32 in the Theory Guide (for )
or Equation 14–42 and Equation 14–43 in the Theory
Guide (for
) to predict
formation
for a gaseous or liquid fuel.
Important: Note that there is a limitation that must be considered when defining more than one liquid fuel stream. See Defining the Fuel Streams for details.
For solid (coal) fuel, ANSYS Fluent will use Equation 14–55 and Equation 14–56 in the Theory Guide (for )
or Equation 14–62 and Equation 14–63 in the Theory
Guide (for
) to predict
formation.
Several inputs are required for the coal fuel
model as follows:
Select the intermediate species (hcn, nh3, or hcn/nh3/no) in the N Intermediate drop-down list.
Specify the mass fraction of nitrogen in the volatiles in the Volatile N Mass Fraction field.
Specify the overall fraction of the volatile , by mass, that will
be converted to the intermediate species and/or product
in
the Conversion Fraction field.
If you selected hcn/nh3/no as
the volatile intermediate, specify the fraction of the
converted volatile
, by mass, that will become hcn and nh3 under Partition Fractions. The fraction of volatile
that will become
will be calculated
by the remainder.
Select the char conversion path from the Char
N Conversion drop-down list as no, hcn, nh3, or hcn/nh3/no. Note that hcn or nh3 can
be selected only if the same species has been selected as the intermediate
species in the N Intermediate drop-down list.
Specify the mass fraction of nitrogen in the char in the Char N Mass Fraction field.
Specify the overall fraction of the char , by mass, that will
be converted to the intermediate species and/or product
in
the Conversion Fraction field.
If you selected hcn/nh3/no as
the char conversion, specify the fraction of the
converted char
, by mass, that will become hcn and nh3 under Partition Fractions. The fraction of char
that will become
will be calculated
by the remainder.
Define the BET internal pore surface area (see BET Surface Area in the Theory Guide for details) of the particles in the BET Surface Area field.
Important: Note that there are limitations that must be considered when defining more than one solid fuel stream. See Defining the Fuel Streams for details.
The following equations are used to determine the mass fraction of nitrogen in the volatiles and char:
(21–2) |
| where | |
|
| |
|
| |
|
|
|
Let | |
|
| |
|
| |
|
| |
|
|
Then the following should hold:
(21–3) |
(21–4) |
(21–5) |
(21–6) |
(21–7) |
The formation of through an
intermediate can be
predicted by two methods. You will specify the method to be used in
the N2O Path tab.
To choose the quasi-steady-state method, select quasi-steady in the N2O Model drop-down list.
Important: The transport equation for the species will not be solved
for
. However,
will be updated at
every iteration. Therefore, the residual values that appear for
are always
zero. Do not be alarmed if the solver keeps printing zero at each
iteration.
To choose the simplified form of the -intermediate
mechanism, select transported-simple in the N2O Model drop-down list. Here, the species
is added to
the list of pollutant species, and its mass fraction is solved via
a transport equation.
The atomic concentration will be calculated according
to the thermal
[O] Model that you have specified previously. If you have not selected the Thermal NOx pathway, then you will be given the option
to specify an [O] Model for the
pathway calculation.
The same three options for the thermal
[O] Model will be the available options.
If you hooked a user-defined function in the Formation tab, you can make a selection in the UDF Rate group box to specify the treatment of the user-defined rate:
Select Replace Fluent Rate to
replace the rate calculated by ANSYS Fluent using
intermediates
with the custom
rate produced by your UDF.
Select Add to Fluent Rate to
add the custom rate produced by your UDF to
the
rate calculated by ANSYS Fluent using
intermediates.
To enable reduction by reburning, click
the Reduction tab in the NOx Model Dialog Box and enable the Reburn option under Methods. In the expanded portion
of the dialog box, as shown in Figure 21.3: The NOx Dialog Box Displaying the Reburn Reduction Method, click the Reburn tab under Reduction Method Parameters, where
you can choose from the following options:
To choose the instantaneous method, select instantaneous [CH] in the Reburn Model drop-down list.
Important: When you use this method, you must be sure to include the species ,
, and
in your problem
definition. See NOx Reduction by Reburning in the Theory
Guide for details.
To choose the partial equilibrium method, select partial-equilibrium in the Reburn Model drop-down list. You then must select the Reburn Fuel Species from the list of available species. ANSYS Fluent will allow you select up to five reburn fuel species. Specify the Equivalent Fuel Type (ch4, ch3, ch2, or ch). For example, if you choose methane as the reburn fuel, then the Equivalent Fuel Type would be ch4. If you choose a reburn fuel such as hv_vol (a volatile component of coal), then you must specify the most appropriate equivalent hydrocarbon fuel type so that the partial equilibrium model will be set up correctly.
Due to coal volatiles behaving very differently, it
is important to select the correct equivalent fuel type. You must
first consider the volatile fuel composition, then check the /
ratio to find the fuel that
most closely matches
,
,
, or
[60]. While the method for best determining the
equivalent fuel is debatable, considering the
/
ratio of the fuel itself is
a reasonable indicator.
Prior to enabling reduction by SNCR, make sure that you have included in the species list nh3 (for reduction by ammonia injection) and co<nh2>2 (for reduction by urea injection). See NOx Reduction by SNCR in the Theory Guide for detailed information about SNCR theory.
To enable reduction by SNCR, click the Reduction tab in the NOx Model Dialog Box and enable the SNCR option under Methods, as shown in Figure 21.4: The NOx Dialog Box Displaying the SNCR Reduction Method.
Then click the SNCR tab under Reduction Method Parameters, where you can choose from the following options:
To have ammonia or urea included as a gas-phase pollutant species from the injection locations, select gaseous in the Injection Method drop-down list.
If you plan to select this option for postprocessing,
then you must also include ammonia or urea as a gas-phase species.
Additionally, you must specify the mass fraction of ammonia or urea
at the respective inlet for the SNCR injection. You must include this
set of inputs prior to the main ANSYS Fluent combustion calculation.
To have ammonia included as a liquid-phase pollutant species from the injection locations, select liquid in the Injection Method drop-down list. If urea is injected as a liquid solution, then select liquid in the Injection Method drop-down list. Note that you must enable the DPM model with urea or ammonia included as a material.
Note: All particle types such as droplets, combusting, and multicomponent particles are compatible with the SNCR model.
If you plan to select this option
for postprocessing, then you must
include
as both a gas-phase and liquid-phase species.
Additionally, you must specify injection locations for liquid droplet
ammonia particles and set gaseous ammonia as the evaporation species.
You must include this set of inputs in conjunction with the main ANSYS Fluent combustion
calculation.
Since urea is a subliming solid, and usually
is injected as a solution, mixed in water, you have to define solid
properties for urea under the Create/Edit Materials Dialog Box. It is assumed that the water
evaporates before urea begins its subliming process. The sublimation
process is modeled similar to the single rate devolatilization model
of coal. You will supply the value for the sublimation rate (). You must specify the water content while defining
the injection properties.
Specify the SNCR Reagent Species as nh3 (ammonia) or co<nh2>2 (urea) in the drop-down list.
When using the non-premixed combustion model with
a liquid-phase reagent injection, enter a value in the Reagent
Fraction in Stream to specify the mass fraction of the
reagent in the reagent stream. The remaining mass fraction is assumed
to be water. If you enabled a secondary stream in your PDF calculation,
by default the secondary stream will act as the reagent stream. You
can assign the primary stream as the reagent stream by using the text
command that follows (enter 0 in response
to the PDF Stream ID prompt that follows
the Injection Method prompt):
define/models/nox-parameters/nox-chemistry
If the Reagent Species selected is co <nh2> 2, then you will either accept the rate-limiting option for Urea Decomposition, or specify the NH3 Conversion value when selecting a user-specified Urea Decomposition.
You will use the urea decomposition under the SNCR tab to define which of the two decomposition models
is to be used. The first model (which is the default) is the rate-limiting
decomposition model, as given in Table 14.3: Two-Step Urea Breakdown Process in the Theory Guide. ANSYS Fluent will
then calculate the source terms according to the rates given in Table 14.3: Two-Step Urea Breakdown Process in
the Theory Guide. The second model is for when you assume that the urea decomposes
instantly into ammonia and at a given proportion. In this
case, you will specify the molar conversion fraction for ammonia,
assuming that the rest of the urea is converted to
. An example value is given above.
The value for user-specified conversion is the mole fraction of
in the mixture
of
and
that is instantly created from
the reagent injection. In this case, there is no urea source because
all of reagent is assumed to convert to both
and
, instantly.
If you want to take into account turbulent fluctuations (as
described in NOx Formation in Turbulent Flows in the Theory
Guide) when you compute the specified formation
(thermal, prompt, and/or fuel, with or without reburn), define the
turbulence parameters in the Turbulence Interaction Mode tab.
Select one of the options in the PDF Mode drop-down list in the Turbulence Interaction Mode tab:
Select temperature to take into account fluctuations of temperature.
Select temperature/species to take into account fluctuations of temperature and mass fraction of the species selected in the Species drop-down list (which appears when you select this option).
(non-premixed and partially premixed combustion calculations only) Select mixture fraction to take into account fluctuation in the mixture fraction(s).
Important: When modeling the formation of other pollutants along with ,
you should compare the selections made in the PDF Mode drop-down lists in the Turbulence Interaction Mode group boxes of the NOx Model Dialog Box and the Turbulence Interaction Mode group boxes of the SOx Model and Soot Model dialog boxes.
If mixture fraction is selected in any of these
dialog boxes, then it must be selected in all of the others as well.
The mixture fraction option is available
only if you are using either the non-premixed or partially premixed
combustion model to model the reacting system. If you use the mixture fraction option, the instantaneous temperatures
and species concentrations are taken from the PDF look-up table as
a function of mixture fraction and enthalpy and the instantaneous rates
are calculated at each cell. The PDF used for convoluting the instantaneous
rates
is the same as the one used to compute the mean flow-field properties.
For example, for single-mixture fraction models the beta PDF is used,
and for two-mixture fraction models, the beta or the double delta
PDF can be used. The PDF for mixture fraction is calculated from the
values of mean mixture fraction and variance at each cell, and the
instantaneous
rates are convoluted with the
mixture fraction PDF to yield the mean rates in turbulent flow.
Note: When mixture fraction is selected
as PDF mode, ANSYS Fluent calculates and tabulates
the rates apriori for faster computations
of
rates. The
rates
are tabulated at the first
iteration and a message
Performing Pollutant PDF integrations...
is displayed in the Fluent console.
If you selected temperature or temperature/species for the PDF Mode, you should define the following parameters in the Turbulence Interaction Mode tab:
allows you to specify the shape of the PDF, which is then integrated to obtain mean rates for the temperature and (if you selected temperature/species for the PDF Mode) the species. If you select beta, the PDF will be modeled using Equation 14–108 in the Theory Guide. If you select gaussian, the PDF will be modeled using Equation 14–111 in the Theory Guide.
allows you to specify the number of points used to integrate the beta or Gaussian function in Equation 14–105 or Equation 14–106 in the Theory Guide on a histogram basis. The default value of 10 is a minimum value. It is recommended that you run the calculation with this minimum value to convergence, and then keep increasing the value (for example, 20–25) until the pollutants of interest stop changing. Increasing this value may improve accuracy, but will also increase the computation time.
allows you to specify the form of transport equation that is solved to calculate the temperature variance. The default selection is algebraic, which is an approximate form of the transport equation (see Equation 14–114 of the Theory Guide). You have the option of selecting transported to instead solve Equation 14–113 in the Theory Guide. Though the transported form is more exact, it is also more expensive computationally.
provides various options for determining the maximum limit of the temperature used for the integration of the PDF (see Equation 8–43 in the Fluent Theory Guide) to calculate mean rates for turbulent fluctuations of NOx:
The default selection is global-tmax, which sets the limit as the maximum temperature in the flow field.
You can select local-tmax if you would rather obtain cell-based maximum temperature limits by multiplying the local cell mean temperature by the value entered in Tmax Factor.
You can select specified-tmax to set the limit for each cell to be the value entered in Tmax.
If you have selected a user-defined function in the NOx Rate drop-down list in the Formation tab, then you can select user-defined so that the temperature limit is specified by a user-defined function. See the Fluent Customization Manual for details about user-defined functions.
only appears if you have selected temperature/species for the PDF Mode. Your selection in this drop-down
menu determines which species’ mass fraction is included in
the formation calculations.
Important: Note that the species variance will always be calculated using the algebraic form of the transport equation (Equation 14–114 in the Theory Guide).
At flow inlet boundaries, you must specify the Pollutant NO Mass Fraction, and if necessary, the Pollutant HCN Mass Fraction, Pollutant NH3 Mass Fraction, and Pollutant N2O Mass Fraction.
Setup →
Boundary Conditions
You can retain the default inlet values of zero for these quantities or you can enter nonzero numbers as appropriate for your combustion system.