# 7.7. Fuego Region

This section is referenced in the following other sections

- Simulation Setup: Averaging
- Simulation Setup: EDC Combustion Model
- Simulation Setup: General Post-Processing
- Simulation Setup: Output Reference
- Simulation Setup: Restart Reference
- Simulation Setup: Source terms
- Simulation Setup: Turbulence Model
- Tutorials: Post-processing

## 7.7.1. Fuego Region

Scope

  Fuego Procedure

Summary

  Contains the commands needed to execute an analysis on this region.

    begin Fuego Region Regionname

       Allow Inverted Elements

       Calculate Mesh Quality Metrics

       Find Maximum Residuals

       Initialize With Continuity Solve

       Integer Data For Subroutine SubName {=} Values...

       Maximum Temperature Allowed From Temperature Extraction {=} Value

       Minimum Temperature Allowed From Temperature Extraction {=} Value

       Nonlinear Residual Plotfile Path {=} Path

       Real Data For Subroutine SubName {=} Values...

       Region Participates In Time Step Selection When Inactive {=} {false | true}

       Set Length Unit Conversion Factor {=} Scale

       Set Mass Unit Conversion Factor {=} Scale

       Set Temperature Units {=} {celsius | fahrenheit | kelvin}

       Set Time Unit Conversion Factor {=} Scale

       Set Unit System To {cgs | mks}

       Setup Warnings Are Errors

       Use Mpmd Radiation [ With {copy} Transfer  ]

       Use Reduced Diffusion Stencil

       Use Simple Radiation Source With Tref {=} Tref And Emissivity {=} Emissivity

       Use Solution Steering With Interval {=} Interval

       Use Finite Element Model ModelName [ Model Coordinates Are Nodal_variable_name  ]

       Warning Level {=} {minor | moderate | severe}

       Initial Uniform Refinement For Num Iterations

       begin Averaging OptionsName
       end

       begin Composite Boundary Condition On Surface Surfacename
       end

       begin Composite Interface Boundary Condition On Surface Surfacename
       end

       begin Fixed Boundary Condition On Surface Surfacename
       end

       begin Heartbeat Label
       end

       begin Heartbeat Output Label
       end

       begin Heat Flux Boundary Condition On Surface Surfacename
       end

       begin History Output Label
       end

       begin Inflow Boundary Condition On Surface Surfacename
       end

       begin Initial Condition Block BlockName
       end

       begin Mass Flux Boundary Condition On Surface Surfacename
       end

       begin Nonconformal Boundary Condition On Surface Surfacename
       end

       begin Open Boundary Condition On Surface Surfacename
       end

       begin Periodic Boundary Condition On Surface Surfacename
       end

       begin Post Process On Surface Surfacename
       end

       begin Postprocess
       end

       begin Restart Data Label
       end

       begin Results Output Label
       end

       begin Solid Object Objectname
       end

       begin Solution Options OptionsName
       end

       begin Symmetry Boundary Condition On Surface Surfacename
       end

       begin Virtual Thermocouple Model On Block BlockName
       end

       begin Wall Boundary Condition On Surface Surfacename
       end

       begin Wall Mass Inject Boundary Condition On Surface Surfacename
       end

    end Fuego Region Regionname

### 7.7.1.1. Line Commands

###### Allow Inverted Elements

Syntax

  Allow Inverted Elements

Summary

  Don’t abort on inverted elements

Description

  Normal behavior will abort on an inverted element. With this beta option on the element volume will be clipped to epsilon with a warning.

###### Calculate Mesh Quality Metrics

Syntax

  Calculate Mesh Quality Metrics

Summary

  Calculates CVFEM mesh quality metrics

Description

  Standard finite element quality metrics may not adequately capture mesh quality for CVFEM. Using this will calculate a mesh quality metric that is based on the distance between the dual volume centroid and the node location, normalized to be nominally between 0 and 100. Lower is better here, so a perfect mesh will have a quality metric of 0. Note that boundary elements have a half control volume which makes this calculation less relevant there, so the quality metric is set to 0 on all boundary nodes.

###### Find Maximum Residuals

Syntax

  Find Maximum Residuals

Summary

  Locate maximum nonlinear equation residual values on the mesh.

Description

  This option will provide the x, y and z location of the maximum nonlinear residual for all equations.

  Note that this option may NOT BE USED WITH Prometheus

###### Initialize With Continuity Solve

Syntax

  Initialize With Continuity Solve

Summary

  Apply a continuity solve to the initial conditions on the first time step

Description

  On the very first time step a continuity solve will be applied to the initial conditions before solving momentum. The solution will proceed in the standard order after that. This option allows initial conditions which may not strictly respect the requirements of incompressibility to be corrected by an initial projection step.

###### Integer Data For Subroutine

Syntax

  Integer Data For Subroutine SubName {=} Values…

Summary

  List of integer data values to be passed down in to the user subroutine. These values may be changed by the user subroutine.

Parameter | Value | Default
--- | --- | ---
SubName | string | –
{=} | {= | are | is} | –
Values | integer… | –

###### Maximum Temperature Allowed From Temperature Extraction

Syntax

  Maximum Temperature Allowed From Temperature Extraction {=} Value

Summary

  Enforce a particular maximum temperature that might occur in temperature extraction from enthalpy and composition.

Description

  This option specifies the maximum temperature to be allowed to be extracted from enthalpy, given the mixture composition. If a temperature is extracted that is greater than this value, a warning will be printed and the temperature will be reset to the previous value.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Value | real | 2600.0 K

###### Minimum Temperature Allowed From Temperature Extraction

Syntax

  Minimum Temperature Allowed From Temperature Extraction {=} Value

Summary

  Enforce a particular minimum temperature that might occur in temperature extraction from enthalpy and composition.

Description

  This option specifies the minimum temperature to be allowed to be extracted from enthalpy, given the mixture composition. If a temperature is extracted that is less than this value, a warning will be printed and the temperature will be reset to the previous value.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Value | real | 250.0 K

###### Nonlinear Residual Plotfile Path

Syntax

  Nonlinear Residual Plotfile Path {=} Path

Summary

  Specify the path to write the nonlinear residual plot files to for this region. Note that all plotfiles will be tagged by the region name as well as the equation name.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Path | string | –

###### Real Data For Subroutine

Syntax

  Real Data For Subroutine SubName {=} Values…

Summary

  List of real data values to be passed down in to the user subroutine. These values may be changed by the user subroutine.

Parameter | Value | Default
--- | --- | ---
SubName | string | –
{=} | {= | are | is} | –
Values | real… | –

###### Region Participates In Time Step Selection When Inactive

Syntax

  Region Participates In Time Step Selection When Inactive {=} {false | true}

Summary

  When region is inactive, it may or may not be able to modify the time step selection

Description

  Fuego can be run with inactivating the region solve. However, the question of how to negotiate the time step remains. If this line command is true, then the last Fuego time step will be provided. However, if this line command is false, Fuego will not participate in time step selection criteria.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
TrueFalse | {false | true} | –

###### Set Length Unit Conversion Factor

Syntax

  Set Length Unit Conversion Factor {=} Scale

Summary

  Specify the conversion factor to convert length units to centimeters

Description

  Fuego allows arbitrary length units to be specified. The user must provide the conversion factor to convert to centimeters. Users should also ensure complete consistency in their input file and mesh - all units should be in the user-specified system.

  Because the default unit system is CGS, use the following convention. If [X] cm = 1 [new length unit], enter “X” for this command. For example, enter 100 if your problem is in meters.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Scale | real | –

###### Set Mass Unit Conversion Factor

Syntax

  Set Mass Unit Conversion Factor {=} Scale

Summary

  Specify the conversion factor to convert mass units to grams

Description

  Fuego allows arbitrary mass units to be specified. The user must provide the conversion factor to convert to grams. Users should also ensure complete consistency in their input file and mesh - all units should be in the user-specified system.

  Because the default unit system is CGS, use the following convention. If [X] g = 1 [new mass unit], enter “X” for this command. For example, enter 1000 if your problem is in kilograms.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Scale | real | –

###### Set Temperature Units

Syntax

  Set Temperature Units {=} {celsius | fahrenheit | kelvin}

Summary

  Specify the scale for temperature units

Description

  Fuego allows the user to select from several temperature scales. Users should also ensure complete consistency in their input file and mesh - all units should be in the user-specified system.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
TempScale | {celsius | fahrenheit | kelvin} | –

###### Set Time Unit Conversion Factor

Syntax

  Set Time Unit Conversion Factor {=} Scale

Summary

  Specify the conversion factor to convert time units to seconds

Description

  Fuego allows arbitrary time units to be specified. The user must provide the conversion factor to convert to seconds. Users should also ensure complete consistency in their input file and mesh - all units should be in the user-specified system.

  Because the default unit system is CGS, use the following convention. If [X] s = 1 [new time unit], enter “X” for this command. For example, enter 60 if your problem is in minutes.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Scale | real | –

###### Set Unit System To

Syntax

  Set Unit System To {cgs | mks}

Summary

  Select a common length-mass-time unit system.

Description

  Shortcut to select meter-kilogram-second (MKS) or centimeter-gram-second unit (CGS) system. This should correspond to the units your mesh and BCs are in. Using Cantera requires a unit conversion, and CGS units are assumed if you do not specify otherwise.

  Explicitly specifying units, either with the “SET UNIT SYSTEM” command or manually with the “SET X UNIT CONVERSION FACTOR” commands also lets Fuego automatically select universal constants like the Stefan-Boltzmann constant, speed of light, and Planck constant (for PMR).

Parameter | Value | Default
--- | --- | ---
UnitSystem | {cgs | mks} | –

###### Setup Warnings Are Errors

Syntax

  Setup Warnings Are Errors

Summary

  Make problem setup warnings be treated as errors.

Description

  By default problem setup warnings are treated as warnings, so things like applying an upwind factor or under-relaxation factor to an equation that isn't active would be a warning.

  By adding this option, things like that will be treated as errors instead of warnings.

###### Use Mpmd Radiation

Syntax

  Use Mpmd Radiation [ With {copy} Transfer ]

Summary

  Use MPMD radiation coupling - requiring other code to communicate with for PMR through MPI

Description

  This solution option indicates that Fuego will be run in MPMD mode, communicating with another executable through MPI for PMR (participating media radiation) coupling. Currently, Nalu is coupled to Fuego for PMR calculations, and several examples exist in the regression test library. Radiation properties (including boundary radiation properties emissivity and transmissivity) are communicated from Fuego to the PMR code through MPMD. Quadrature rules, radiation mesh, and radiation solver settings are specified in the input deck for that executable. Fuego and the MPMD coupled PMR code are executed simultaneously as:

  mpirun -n nF fuego -i fuego.i : -n nN nalu -i nalu.i (Nalu)

  where nF, nN, are the integer numbers of processors to be used for Fuego and Nalu, respectively. fuego.i and nalu.i are the Fuego and Nalu input decks, respectively.

  By default it is assumed the Fuego and PMR meshes are different and a general interpolative MPMD transfer will be used. If the meshes are static and identical, a user may instead specify to use a more efficient COPY transfer. COPY transfers are not supported if the fluid side undergoes mesh refinement or there is mesh motion.

###### Use Reduced Diffusion Stencil

Syntax

  Use Reduced Diffusion Stencil

Summary

  Use canonical seven point diffusion stencil

Description

  The standard diffusion operator supported is represented by the twenty seven node canonical hexahedron stencil. This option allows for all diffusion operators to reduce to the canonical seven point stencil (again hexahedron) by shifting integration point evaluation from the sub surface control volume face centroid to the edge centroid.

  This option may be beneficial to use on a highly skewed mesh.

###### Use Simple Radiation Source With Tref

Syntax

  Use Simple Radiation Source With Tref {=} Tref And Emissivity {=} Emissivity

Summary

  Use a difference between the and to approximate radiation to the far field.

Description

  Calculates the scalar_flux term as rather than using a PMR solver.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Tref | real | –
{=} | {= | are | is} | –
Emissivity | real | –

###### Use Solution Steering With Interval

Syntax

  Use Solution Steering With Interval {=} Interval

Summary

  Change parameters interactively

Description

  Create a solution steering file with parameters that the user can interactively modify during the course of a solution. The file is automatically written during the simulation with the options that are allowed to change. It is read and written again based on the interval set initially in the input file and potentially modified in the steering file. The interval defines how often the file gets read (number of time steps).

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Interval | integer | 1

###### Use Finite Element Model

Syntax

  Use Finite Element Model ModelName [ Model Coordinates Are Nodal_variable_name ]

Summary

  Associates a predefined finite element model with this region.

Parameter | Value | Default
--- | --- | ---
ModelName | string | –

###### Warning Level

Syntax

  Warning Level {=} {minor | moderate | severe}

Summary

  Set the runtime warning output level.

Description

  Control output level of runtime warnings. Choose MINOR (default) to output all warnings, MODERATE to output moderate or severe warnings only, and SEVERE to output only severe errors.

  Examples of MINOR errors are mass fractions slightly outside the 0 to 1 range and turbulent production to dissipation ratio clipping.

  Examples of MODERATE errors are temperature extraction hitting the clipping bounds or mass fractions farther outside the 0 to 1 bounds (greater than 10 percent out of bounds).

  Examples of SEVERE errors are temperature extraction failures or linear solver failures.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
WarningLevel | {minor | moderate | severe} | –

###### Initial Uniform Refinement For

Syntax

  Initial Uniform Refinement For Num Iterations

Summary

  Refine for n number of iterations on initialization

Parameter | Value | Default
--- | --- | ---
Num | integer | –

## 7.7.2. Averaging

Scope

  Fuego Region

Summary

  Specify information regarding the Reynolds and Favre averaging. The Reynolds average is the time average of a value:

  where is the quantity of interest at time and the integration is over , the time interval which is averaged.

  The Favre average is the ratio of two Reynolds averages:

  Where is the quantity of interest and mass is the mass.

    begin Averaging OptionsName

       Butterworth A Coefficients {=} Coeffs...

       Butterworth B Coefficients {=} Coeffs...

       Butterworth Filtered Field RegisteredField As AverageField [ On Output Block BlockName  ]

       Butterworth Time Step {=} TimeStep

       Compute {modeled_reynolds_stress | modeled_scalar_flux | resolved_dissipation | resolved_favre_stress | resolved_production | resolved_reynolds_stress | resolved_scalar_flux | resolved_turbulent_kinetic_energy} [ Of FieldName  ]

       Favre Average Field RegisteredField As AverageField [ On Output Block BlockName  ]

       Log Output

       Moving Average Filtered Field RegisteredField As AverageField [ On Output Block BlockName  ]

       Moving Average Time {=} emaCharTime

       Reset Filter On Restart

       Reynolds Average Field RegisteredField As AverageField [ On Output Block BlockName  ]

       Starting Time {=} StartingTime

       Time Interval Length {=} IntervalLength

    end Averaging OptionsName

### 7.7.2.1. Line Commands

###### Butterworth A Coefficients

Syntax

  Butterworth A Coefficients {=} Coeffs…

Summary

  A coefficients for the Butterworth filter

Description

  The list of A coefficients for the butterworth filter. See the BUTTERWORTH FILTERED FIELD command documentation for details.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Coeffs | real… | –

###### Butterworth B Coefficients

Syntax

  Butterworth B Coefficients {=} Coeffs…

Summary

  B coefficients for the Butterworth filter

Description

  The list of B coefficients for the butterworth filter. See the BUTTERWORTH FILTERED FIELD command documentation for details.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Coeffs | real… | –

###### Butterworth Filtered Field

Syntax

  Butterworth Filtered Field RegisteredField As AverageField [ On Output Block BlockName ]

Summary

  Generates Butterworth filter of field.

Description

  The Butterworth filter operations assume that the data is given at a constant time step. The actual time step may vary during the analysis depending on the time stepping mode. The `BUTTERWORTH TIME STEP` command is used to linearly interpolate the data being produced at a non-constant time step down to some specified constant time step. The interpolation time step must be larger than zero and ideally should be specified to be smaller than the smallest time step with which the computations will iterate.

  One way to obtain the filtering coefficients is with MATLAB. The following is an example of defining a third order Butterworth filter with a pass frequency of 100Hz at data interpolated to a time step of seconds. The filter is then used to filter acceleration histories of the nodes to 100Hz. The MATLAB code below will give the desired filtering coefficients. The full 16-digit precision of the coefficients returned by MATLAB should be used. If truncated precision numbers are used, the filters can potentially be unstable.

      clear;
      format long e;
      passFrequency = 100;
      interp_ts = 1.0e-5;
      butterCoeff = 2.0*interp_ts*passFrequency;
      [bcoeff,acoeff] = butter(3,butterCoeff);
      acoeff
      bcoeff

  The computed filtering coefficients can be used in the averaging block as show below. If the analysis time step always remains above the filter will be valid. If the analysis time step drops below there could be aliasing issues, and a smaller interpolation time step should be specified.

      BUTTERWORTH A COEFFICIENTS = 1.000000000000000e+00 -2.987433650055722e+00 \$
                 2.974946132665442e+00 -9.875122361107358e-01
      BUTTERWORTH B COEFFICIENTS = 3.081237301416628e-08  9.243711904249885e-08 \$
                 9.243711904249885e-08  3.081237301416628e-08
      BUTTERWORTH TIME STEP = 1e-5

  Start time and time interval length commands are not used in the Butterworth filter.

Parameter | Value | Default
--- | --- | ---
RegisteredField | string | –
AverageField | string | –

###### Butterworth Time Step

Syntax

  Butterworth Time Step {=} TimeStep

Summary

  Time step for butterworth filter.

Description

  The time step for the butterworth filter. See the BUTTERWORTH FILTERED FIELD command documentation for details.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
TimeStep | real | 0.0

###### Compute

Syntax

  Compute {modeled_reynolds_stress | modeled_scalar_flux | resolved_dissipation | resolved_favre_stress | resolved_production | resolved_reynolds_stress | resolved_scalar_flux | resolved_turbulent_kinetic_energy} [ Of FieldName ]

Summary

  Compute a modeled or resolved derived quantity.

Description

  Select from several pre-defined quantities to compute, described in the list below:

  RESOLVED_REYNOLDS_STRESS

  RESOLVED_FAVRE_STRESS

  RESOLVED_TURBULENT_KINETIC_ENERGY

  RESOLVED_PRODUCTION

  RESOLVED_DISSIPATION

  RESOLVED_SCALAR_FLUX

  MODELED_REYNOLDS_STRESS

  MODELED_SCALAR_FLUX

Parameter | Value | Default
--- | --- | ---
Type | {modeled_reynolds_stress | modeled_scalar_flux | resolved_dissipation | resolved_favre_stress | resolved_production | resolved_reynolds_stress | resolved_scalar_flux | resolved_turbulent_kinetic_energy} | –

###### Favre Average Field

Syntax

  Favre Average Field RegisteredField As AverageField [ On Output Block BlockName ]

Summary

  Generates Favre average of field.

Description

  The Favre average is the ratio of two Reynolds averages:

  Where is the quantity of interest and is the mass.

  The field to be averaged must exist in the model being solved. The averaged field will be created and output on the specified block. It the block is not specified, the average will be defined and output on any nodes that the base field exists.

  Since the Reynolds average of the mass and the Reynolds average of the field to be Favre averaged must be computed in order to calculate the ratio, these two extra fields will be created and written to the results file. The Reynolds averaged mass is available as “density_Avg” and the Reynolds average of the mass weighted Favre field, , will be available as the specified output field name in this line command appended by the string “_Wtd”.

Parameter | Value | Default
--- | --- | ---
RegisteredField | string | –
AverageField | string | –

###### Log Output

Syntax

  Log Output

Summary

  Activate verbose logging for filters

Description

  When this option is on, additional logging will be output to the log file for each filter, including resets, filter time, and filter active/inactive state.

###### Moving Average Filtered Field

Syntax

  Moving Average Filtered Field RegisteredField As AverageField [ On Output Block BlockName ]

Summary

  Generates an exponential moving average filter.

Description

  The moving average filter uses an exponential moving average to update the averaging field () using the source field () and a blending coefficient ():

  The filter time () is defined using the `MOVING AVERAGE TIME` command.

Parameter | Value | Default
--- | --- | ---
RegisteredField | string | –
AverageField | string | –

###### Moving Average Time

Syntax

  Moving Average Time {=} emaCharTime

Summary

  The characteristic filter time to use for the moving average filter.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
emaCharTime | real | 0.0

###### Reset Filter On Restart

Syntax

  Reset Filter On Restart

Summary

  Reset Favre/Reynolds averages specified in block

Description

  This option, on restart, will remove history from averages, restarting the average if the current time > start time of the average. This option is not compatible with Butterworth filtering.

###### Reynolds Average Field

Syntax

  Reynolds Average Field RegisteredField As AverageField [ On Output Block BlockName ]

Summary

  Generates Reynolds average of field.

Description

  The Reynolds average is the time average of a value:

  where is the quantity of interest at time and the integral is evaluated over , the time interval which is averaged.

  The field to be averaged must exist in the model being solved. The averaged field will be created and output on the specified block. It the block is not specified, the average will be defined and output on any nodes that the base field exists.

  Since the Reynolds average of the mass and the Reynolds average of the field to be Favre averaged must be computed in order to calculate the ratio, these two extra fields will be created and written to the results file. The Reynolds averaged mass is available as “density_Avg” and the Reynolds average of the mass weighted Favre field, , will be available as the specified output field name in the line command appended by the string “_Wtd”.

Parameter | Value | Default
--- | --- | ---
RegisteredField | string | –
AverageField | string | –

###### Starting Time

Syntax

  Starting Time {=} StartingTime

Summary

  Time for which the averaging starts.

Description

  If the starting time is specified then the averaging will not start until the starting time is obtained. All data before the starting time will be ignored and the average will be zero. Once the starting time is reached the averaging will proceed as described under the time interval length parameter with intervals over where is the starting time.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
StartingTime | real | 0.0

###### Time Interval Length

Syntax

  Time Interval Length {=} IntervalLength

Summary

  Time interval length over which average is computed.

Description

  If the time interval length is specified as , The Reynolds or Favre averages specified will be determined over intervals of length . The intervals will be over for integers . At the end of one interval, the running average that is being computed will be zeroed out and the averaging starting all over again. This means that soon after an interval change the output field will contain just the average from the beginning of that time interval to the current time. The result is that at every interval boundary there is liable to be a jump or variation in the running average that will be smoothed out over time.

  If the starting time parameter is specified then the averaging will not start until the starting time is obtained. All data before the starting time will be ignored and the average will be zero. Once the starting time is reached the averaging will proceed as described with intervals over where is the starting time.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
IntervalLength | real | REAL_MAX

## 7.7.3. Heartbeat

Scope

  Average Region, Fuego Region, Input_Output Region, Particle Region

Summary

  Describes the location and type of the output stream used for outputting the heartbeat information for the enclosing region.

    begin Heartbeat Label

       Additional Steps {=} List_of_steps...

       Additional Times {=} List_of_times...

       Append {=} {false | off | on | true}

       At Step n {increment | interval} {=} m

       At Time Dt1 {increment | interval} {=} Dt2

       Auto Output {all | element | global | nodal} User Defined Variables [ In UserOutputHeartBeatList...  ]

       Element [ VariableList...  ]

       Exists {=} {abort | append | overwrite}

       Face [ VariableList...  ]

       Format {=} {csv | original | spyhis}

       Global [ Variables...  ]

       Labels {=} {off | on}

       Legend {=} {off | on}

       Monitor {= | the} {history | restart | results}

       Nodal [ VariableList...  ]

       Node [ VariableList...  ]

       Nodeset [ VariableList...  ]

       Output On Signal {=} {sigabrt | sigalrm | sigfpe | sighup | sigill | sigint | sigkill | sigpipe | sigquit | sigsegv | sigterm | sigusr1 | sigusr2}

       Precision {=} Precision

       Start Time {=} Start_time

       Stream Name {=} OutputFilename

       Synchronize Output

       Termination Time {=} Final_time

       Timestamp Format

       Timestep Adjustment Interval {=} Nsteps

       Use Output Scheduler Timer_name

       Variable {=} {edge | element | face | global | nodal | node} Variable_list...

    end Heartbeat Label

### 7.7.3.1. Line Commands

###### Additional Steps

Syntax

  Additional Steps {=} List_of_steps…

Summary

  Additional simulation steps when output should occur.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
List_of_steps | integer… | –

###### Additional Times

Syntax

  Additional Times {=} List_of_times…

Summary

  Additional simulation times when output should occur.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
List_of_times | real… | –

###### Append

Syntax

  Append {=} {false | off | on | true}

Summary

  Specifies whether the heartbeat file is appended if it exists. By default, the file is appended if restart is requested and not if restart is not requested. This option does not work for automatic restarts because a new heartbeat file is written with each auto restart.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Option | {false | off | on | true} | –

###### At Step

Syntax

  At Step n {increment | interval} {=} m

Summary

  Specify an output interval in terms of the internal iteration step count. The first step specifies the step count at the beginning of this interval and the second step specifies the output frequency to be used within this interval.

Parameter | Value | Default
--- | --- | ---
n | integer | –
Option | {increment | interval} | –
{=} | {= | are | is} | –
m | integer | –

###### At Time

Syntax

  At Time Dt1 {increment | interval} {=} Dt2

Summary

  Specify an output interval in terms of the internal simulation time. The first time specifies the time at the beginning of this time interval and the second time specifies the output frequency to be used within this interval.

Parameter | Value | Default
--- | --- | ---
Dt1 | real | –
Option | {increment | interval} | –
{=} | {= | are | is} | –
Dt2 | real | –

###### Auto Output

Syntax

  Auto Output {all | element | global | nodal} User Defined Variables [ In UserOutputHeartBeatList… ]

Summary

  Allows users to automatically output all user output defined variables for the type requested.

Parameter | Value | Default
--- | --- | ---
auto_output_type_4 | {all | element | global | nodal} | –

###### Element

Syntax

  Element [ VariableList… ]

Summary

  Define the element variables that should be written to the heartbeat database. The syntax is: “element {internal_name} at element {id} as {DBname}” or “element {internal_name} nearest location X, Y, Z as {DBname}”.

  Where {internal_name} is the name of the variable in the Sierra application; and {DBname} is the name as it should appear on the heartbeat database.

###### Exists

Syntax

  Exists {=} {abort | append | overwrite}

Summary

  Specify the behavior when creating this database and there is an existing file with the same name. The default behavior is “OVERWRITE” which deletes the existing file and creates a new file of the same name. “APPEND” will (if possible) append the new data to the end of the existing file. “ABORT” will print an error message and end the analysis.

Parameter | Value | Default
--- | --- | ---
{=} | {= | is} | –
Option2 | {abort | append | overwrite} | –

###### Face

Syntax

  Face [ VariableList… ]

Summary

  Define the face variables that should be written to the heartbeat database. The syntax is: “face {internal_name} at face {id} as {DBname}” or “face {internal_name} nearest location X, Y, Z as {DBname}”.

  Where {internal_name} is the name of the variable in the Sierra application; and {DBname} is the name as it should appear on the heartbeat database.

###### Format

Syntax

  Format {=} {csv | original | spyhis}

Summary

  The stream type/format to be used for the output results.The only three options at this time are ‘Original’ which is the old default Sierra heartbeat format; ‘SpyHis’ which mimics the CTH Spyhis history output format; and ‘CSV’

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
StreamTypes | {csv | original | spyhis} | –

###### Global

Syntax

  Global [ Variables… ]

Summary

  Define the global/reduction variables that should be written to the heartbeat database. The syntax is: “global {internal_name} as {DBname}”.

  Where {internal_name} is the name of the variable in the Sierra application; and {DBname} is the name as it should appear on the heartbeat database.

###### Labels

Syntax

  Labels {=} {off | on}

Summary

  Specifies whether labels will be displayed or just the value of the variable. Labels will be shown if this line is not present.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Option | {off | on} | on

###### Legend

Syntax

  Legend {=} {off | on}

Summary

  Specifies whether a legend will be displayed prior to outputting any variables. The legend will not be shown unless this line is present. The legend shows the names of the variables that will be written to the heartbeat output stream. If the variable has multiple components, then the component count is shown after the variable e.g., velocity(3).

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Option | {off | on} | on

###### Monitor

Syntax

  Monitor {= | the} {history | restart | results}

Summary

  Specifies whether a line will be written to the heartbeat stream when either the results, history, and/or restart data are output.

Parameter | Value | Default
--- | --- | ---
Equals | {= | the} | –
Option | {history | restart | results} | –

###### Nodal

Syntax

  Nodal [ VariableList… ]

Summary

  Define the nodal variables that should be written to the heartbeat database. The syntax is: “nodal {internal_name} at node {id} as {DBname}” or “nodal {internal_name} nearest location X, Y, Z as {DBname}”.

  Where {internal_name} is the name of the variable in the Sierra application; and {DBname} is the name as it should appear on the heartbeat database.

###### Node

Syntax

  Node [ VariableList… ]

Summary

  Define the nodal variables that should be written to the heartbeat database. The syntax is: “node {internal_name} at node {id} as {DBname}” or “node {internal_name} nearest location X, Y, Z as {DBname}”.

  Where {internal_name} is the name of the variable in the Sierra application; and {DBname} is the name as it should appear on the heartbeat database.

###### Nodeset

Syntax

  Nodeset [ VariableList… ]

Summary

  Define the nodeset variables that should be written to the heartbeat database. The syntax is: “nodeset {internal_name} at node {id} as {DBname}” or “nodeset {internal_name} nearest location X, Y, Z as {DBname}”.

  Where {internal_name} is the name of the variable in the Sierra application; and {DBname} is the name as it should appear on the heartbeat database. This option finds a single value for the {internal_name} specified without having to specify a nodeset id or name.

###### Output On Signal

Syntax

  Output On Signal {=} {sigabrt | sigalrm | sigfpe | sighup | sigill | sigint | sigkill | sigpipe | sigquit | sigsegv | sigterm | sigusr1 | sigusr2}

Summary

  When the specified signal is raised, the output stream associated with this block will be output.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Signals | {sigabrt | sigalrm | sigfpe | sighup | sigill | sigint | sigkill | sigpipe | sigquit | sigsegv | sigterm | sigusr1 | sigusr2} | –

###### Precision

Syntax

  Precision {=} Precision

Summary

  The precision to be used for the output of real variables (default=5).

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Precision | integer | 5

###### Start Time

Syntax

  Start Time {=} Start_time

Summary

  Specify the time to start outputting results from this output request block. This time overrides all ‘at time’ and ‘at step’ specifications.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Start_time | real | –

###### Stream Name

Syntax

  Stream Name {=} OutputFilename

Summary

  The filename of where the heartbeat data should be written. If the filename begins with the ‘/’ character, it is an absolute path; otherwise, the path to the current directory will be prepended to the name. In addition, there are several predefined streams that can be specified. The predefined streams are ‘cout’ or ‘stdout’ specifies standard output; ‘cerr’, ‘stderr’, ‘clog’, or ‘log’ specifies standard error; ‘output’ or ‘outputP0’ specifies Sierra’s standard output which is redirected to the file specified by the ‘-o’ option on the command line. If the file already exists, it is overwritten. If this line is omitted, then a filename will be created from the basename of the input file with a “.hrt” suffix appended.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
OutputFilename | string | –

###### Synchronize Output

Syntax

  Synchronize Output

Summary

  In an analysis with multiple regions, it is sometimes desirable to synchronize the output of results data between the regions. This can be done by adding the SYNCHRONIZE OUTPUT command line to the results output block. If a results block has this set, then it will write output whenever a previous region writes output. The ordering of regions is based on the order in the input file, algorithmic considerations, or by solution control specifications.

  Although the USE OUTPUT SCHEDULER command line can also synchronize output between regions, the SYNCHRONIZE OUTPUT command line will synchronize the output with regions where the output frequency is not under the direct control of the Sierra IO system. Examples of this are typically coupled applications where one or more of the codes are not Sierra-based applications such as Alegra and CTH. A results block with SYNCHRONIZE OUTPUT specified will also synchronize its output with the output of the external code.

  The SYNCHRONIZE OUTPUT command can be used with other output scheduling commands such as time-based or step-based output specifications.

###### Termination Time

Syntax

  Termination Time {=} Final_time

Summary

  Specify the time to stop outputting results from this output request block.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Final_time | real | –

###### Timestamp Format

Syntax

  Timestamp Format

Summary

  The format to be used for the timestamp. See ‘man strftime’ for more information.

###### Timestep Adjustment Interval

Syntax

  Timestep Adjustment Interval {=} Nsteps

Summary

  Specify the number of steps to ‘look ahead’ and adjust the timestep to ensure that the specified output times or simulation end time will be hit ‘exactly’.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Nsteps | integer | –

###### Use Output Scheduler

Syntax

  Use Output Scheduler Timer_name

Summary

  Associates a predefined output scheduler with this output block (results, restart, heartbeat, or history).

Parameter | Value | Default
--- | --- | ---
Timer_name | string | –

###### Variable

Syntax

  Variable {=} {edge | element | face | global | nodal | node} Variable_list…

Summary

  Define the variables that should be written to the heartbeat output. The user can request that the values of certain variables be output on the heartbeat line. These variables are limited to region and framework control data currently. The syntax is:

      variable = {entity_type} {internal_name} at
                 {entity_type} {entity_id}     as {external_name}
      variable = {entity_type} {internal_name} nearest location
                 {x,y,z} as {external_name}

  For global variables, use:

      variable = global {internal_name} [as {external_name}]

  Where:

      entity_type = node, element, face, edge, global
      internal_name = Sierra variable name
      entity_id = id of the node, element, face, edge that you want
              the specified variable output at.
      external_name = name of variable on the database.

  The names ‘timestep’, and ‘time’ can be specified as variables also. They are the current timestep and simulation time. This line can appear multiple times.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Option | {edge | element | face | global | nodal | node} | –
Variable_list | string… | –

## 7.7.4. History Output

Scope

  Average Region, Fuego Region, Input_Output Region, Particle Region

Summary

  Describes the location and type of the output stream used for outputting history for the enclosing region.

    begin History Output Label

       Additional Steps {=} List_of_steps...

       Additional Times {=} List_of_times...

       At Step n {increment | interval} {=} m

       At Time Dt1 {increment | interval} {=} Dt2

       Auto Output {all | element | global | nodal} User Defined Variables [ In UserOutputHistoryList...  ]

       Database Name {=} StreamName

       Database Type {=} {catalyst | catalyst_exodus | cgns | dof | dof_exodus | exodus | exodusii | exonull | generated | genesis | null | parallel_exodus | textmesh}

       Element [ VariableList...  ]

       Exists {=} {abort | add_suffix | append | overwrite}

       Face [ VariableList...  ]

       Flush Interval {=} Option

       Global [ Variables...  ]

       Nodal [ VariableList...  ]

       Node [ VariableList...  ]

       Nodeset [ VariableList...  ]

       Output On Signal {=} {sigabrt | sigalrm | sigfpe | sighup | sigill | sigint | sigkill | sigpipe | sigquit | sigsegv | sigterm | sigusr1 | sigusr2}

       Overwrite {=} {false | no | off | on | true | yes}

       Property PropertyName {=} PropertyValue

       Start Time {=} Start_time

       Synchronize Output

       Termination Time {=} Final_time

       Timestep Adjustment Interval {=} Nsteps

       Title

       Use Dynamic Topology Io

       Use Output Scheduler Timer_name

       Variable {=} {edge | element | face | global | nodal | node} Variable_list...

    end History Output Label

### 7.7.4.1. Line Commands

###### Additional Steps

Syntax

  Additional Steps {=} List_of_steps…

Summary

  Additional simulation steps when output should occur.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
List_of_steps | integer… | –

###### Additional Times

Syntax

  Additional Times {=} List_of_times…

Summary

  Additional simulation times when output should occur.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
List_of_times | real… | –

###### At Step

Syntax

  At Step n {increment | interval} {=} m

Summary

  Specify an output interval in terms of the internal iteration step count. The first step specifies the step count at the beginning of this interval and the second step specifies the output frequency to be used within this interval.

Parameter | Value | Default
--- | --- | ---
n | integer | –
Option | {increment | interval} | –
{=} | {= | are | is} | –
m | integer | –

###### At Time

Syntax

  At Time Dt1 {increment | interval} {=} Dt2

Summary

  Specify an output interval in terms of the internal simulation time. The first time specifies the time at the beginning of this time interval and the second time specifies the output frequency to be used within this interval.

Parameter | Value | Default
--- | --- | ---
Dt1 | real | –
Option | {increment | interval} | –
{=} | {= | are | is} | –
Dt2 | real | –

###### Auto Output

Syntax

  Auto Output {all | element | global | nodal} User Defined Variables [ In UserOutputHistoryList… ]

Summary

  Allows users to automatically output all user output defined variables for the type requested.

Parameter | Value | Default
--- | --- | ---
auto_output_type_2 | {all | element | global | nodal} | –

###### Database Name

Syntax

  Database Name {=} StreamName

Summary

  The base name of the database containing the output history. If the filename begins with the ‘/’ character, it is an absolute path; otherwise, the path to the current directory will be prepended to the name. If this line is omitted, then a filename will be created from the basename of the input file with a “.h” suffix appended.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
StreamName | string | –

###### Database Type

Syntax

  Database Type {=} {catalyst | catalyst_exodus | cgns | dof | dof_exodus | exodus | exodusii | exonull | generated | genesis | null | parallel_exodus | textmesh}

Summary

  The database type/format to be used for the output history.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
DatabaseTypes | {catalyst | catalyst_exodus | cgns | dof | dof_exodus | exodus | exodusii | exonull | generated | genesis | null | parallel_exodus | textmesh} | –

###### Element

Syntax

  Element [ VariableList… ]

Summary

  Define the element variables that should be written to the history database. The syntax is: “element {internal_name} at element {id} as {DBname}” or “element {internal_name} nearest location X, Y, Z as {DBname}”.

  Where {internal_name} is the name of the variable in the Sierra application; and {DBname} is the name as it should appear on the history database.

###### Exists

Syntax

  Exists {=} {abort | add_suffix | append | overwrite}

Summary

  Specify the behavior when creating this database and there is an existing file with the same name. The default behavior is “OVERWRITE” which deletes the existing file and creates a new file of the same name. “APPEND” will (if possible) append the new data to the end of the existing file. “ABORT” will print an error message and end the analysis. “ADD_SUFFIX” will add a -s???? suffix where the ???? is replaced by a sequential number starting at 0002.

Parameter | Value | Default
--- | --- | ---
{=} | {= | is} | –
Option2 | {abort | add_suffix | append | overwrite} | –

###### Face

Syntax

  Face [ VariableList… ]

Summary

  Define the face variables that should be written to the history database. The syntax is: “face {internal_name} at face {id} as {DBname}” or “face {internal_name} nearest location X, Y, Z as {DBname}”.

  Where {internal_name} is the name of the variable in the Sierra application; and {DBname} is the name as it should appear on the history database.

###### Flush Interval

Syntax

  Flush Interval {=} Option

Summary

  The minimum time interval (in seconds) at which output will be explicitly flushed to disk. The default is 10 seconds.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Option | integer | 10

###### Global

Syntax

  Global [ Variables… ]

Summary

  Define the global/reduction variables that should be written to the history database. The syntax is: “global {internal_name} as {DBname}”.

  Where {internal_name} is the name of the variable in the Sierra application; and {DBname} is the name as it should appear on the history database.

###### Nodal

Syntax

  Nodal [ VariableList… ]

Summary

  Define the nodal variables that should be written to the history database. The syntax is: “nodal {internal_name} at node {id} as {DBname}” or “nodal {internal_name} nearest location X, Y, Z as {DBname}”.

  Where {internal_name} is the name of the variable in the Sierra application; and {DBname} is the name as it should appear on the history database.

###### Node

Syntax

  Node [ VariableList… ]

Summary

  Define the nodal variables that should be written to the history database. The syntax is: “node {internal_name} at node {id} as {DBname}” or “node {internal_name} nearest location X, Y, Z as {DBname}”.

  Where {internal_name} is the name of the variable in the Sierra application; and {DBname} is the name as it should appear on the history database.

###### Nodeset

Syntax

  Nodeset [ VariableList… ]

Summary

  Define the nodeset variables that should be written to the history database. The syntax is: “nodeset {internal_name} at node {id} as {DBname}” or “nodeset {internal_name} nearest location X, Y, Z as {DBname}”.

  Where {internal_name} is the name of the variable in the Sierra application; and {DBname} is the name as it should appear on the history database.

###### Output On Signal

Syntax

  Output On Signal {=} {sigabrt | sigalrm | sigfpe | sighup | sigill | sigint | sigkill | sigpipe | sigquit | sigsegv | sigterm | sigusr1 | sigusr2}

Summary

  When the specified signal is raised, the output stream associated with this block will be output.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Signals | {sigabrt | sigalrm | sigfpe | sighup | sigill | sigint | sigkill | sigpipe | sigquit | sigsegv | sigterm | sigusr1 | sigusr2} | –

###### Overwrite

Syntax

  Overwrite {=} {false | no | off | on | true | yes}

Summary

  (DEPRECATED, Use EXISTS) Specify whether the database should be overwritten if it exists. The default behavior is to overwrite unless this command is specified in the output block and either off, false, or no is specified.

Parameter | Value | Default
--- | --- | ---
{=} | {= | is} | –
Option2 | {false | no | off | on | true | yes} | –

###### Property

Syntax

  Property PropertyName {=} PropertyValue

Summary

  Define a database property named “PropertyName” with the value “PropertyValue”. If PropertyValue consists of all digits, it will define an integer property. If PropertyValue is “true” or “yes” or “false” or “no”, it will define a logical property; otherwise it will define a string property. Supported properties are typically database dependent; Some history-related properties are:

  - VARIABLE_NAME_CASE = upper|lower

  - MAX_NAME_LENGTH = value (32)

Parameter | Value | Default
--- | --- | ---
PropertyName | string | –
{=} | {= | are | is} | –
PropertyValue | string | –

###### Start Time

Syntax

  Start Time {=} Start_time

Summary

  Specify the time to start outputting results from this output request block. This time overrides all ‘at time’ and ‘at step’ specifications.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Start_time | real | –

###### Synchronize Output

Syntax

  Synchronize Output

Summary

  In an analysis with multiple regions, it is sometimes desirable to synchronize the output of results data between the regions. This can be done by adding the SYNCHRONIZE OUTPUT command line to the results output block. If a results block has this set, then it will write output whenever a previous region writes output. The ordering of regions is based on the order in the input file, algorithmic considerations, or by solution control specifications.

  Although the USE OUTPUT SCHEDULER command line can also synchronize output between regions, the SYNCHRONIZE OUTPUT command line will synchronize the output with regions where the output frequency is not under the direct control of the Sierra IO system. Examples of this are typically coupled applications where one or more of the codes are not Sierra-based applications such as Alegra and CTH. A results block with SYNCHRONIZE OUTPUT specified will also synchronize its output with the output of the external code.

  The SYNCHRONIZE OUTPUT command can be used with other output scheduling commands such as time-based or step-based output specifications.

###### Termination Time

Syntax

  Termination Time {=} Final_time

Summary

  Specify the time to stop outputting results from this output request block.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Final_time | real | –

###### Timestep Adjustment Interval

Syntax

  Timestep Adjustment Interval {=} Nsteps

Summary

  Specify the number of steps to ‘look ahead’ and adjust the timestep to ensure that the specified output times or simulation end time will be hit ‘exactly’.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Nsteps | integer | –

###### Title

Syntax

  Title

Summary

  Specify the title to be used for this specific output block.

###### Use Dynamic Topology Io

Syntax

  Use Dynamic Topology Io

Summary

  Specify that the app use IO for dynamic topology modifications where the output files are stored in a single database. Legacy file format for dynamically changing topology results in the creation of multiple files for each output on a mesh modification. This option leverages the ability of netCDF to create mesh groups within a single database and concatenate all mesh files into one. The names of each mesh group are of the form IOSS_MESH_GROUP-??? where ??? is the 1-based output index 1, 2, …, 10, …., 100, … Please note that netCDF has a current limit of 65,536 groups

###### Use Output Scheduler

Syntax

  Use Output Scheduler Timer_name

Summary

  Associates a predefined output scheduler with this output block (results, restart, heartbeat, or history).

Parameter | Value | Default
--- | --- | ---
Timer_name | string | –

###### Variable

Syntax

  Variable {=} {edge | element | face | global | nodal | node} Variable_list…

Summary

  Define the variables that should be written to the history database. The syntax is: “variable = entity {internal_name} at entity {id} as {DBname}” or “variable = entity {internal_name} nearest location X, Y, Z as {DBname}” or “variable = entity {internal_name} at location X, Y, Z as {DBname}”.

  Where {entity} is ‘node’, ‘element’, ‘face’, or ‘edge’; {internal_name} is the name of the variable in the Sierra application; and {DBname} is the name as it should appear on the history database.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Option | {edge | element | face | global | nodal | node} | –
Variable_list | string… | –

## 7.7.5. Restart Data

Scope

  Average Region, Fuego Region, Input_Output Region, Particle Region

Summary

  Describes the data required to output and input restart data for the enclosing region.

    begin Restart Data Label

       Additional Steps {=} List_of_steps...

       Additional Times {=} List_of_times...

       At Step n {increment | interval} {=} m

       At Time Dt1 {increment | interval} {=} Dt2

       At Wall Time Dt1 {increment | interval} {=} Dt2

       Component Separator Character {=} Separator

       Cycle Count {=} Count

       Database Name {=} StreamName

       Database Type {=} {catalyst | catalyst_exodus | cgns | dof | dof_exodus | exodus | exodusii | exonull | generated | genesis | null | parallel_exodus | textmesh}

       Debug Dump

       Decomposition Method {=} {block | cyclic | external | geom_kway | hsfc | kway | kway_geom | linear | map | metis_sfc | random | rcb | rib | variable}

       Exists {=} {abort | add_suffix | append | overwrite}

       File Cycle Count {=} Count

       Flush Interval {=} Option

       Input Database Name {=} StreamName

       Optional

       Output Database Name {=} StreamName

       Output On Signal {=} {sigabrt | sigalrm | sigfpe | sighup | sigill | sigint | sigkill | sigpipe | sigquit | sigsegv | sigterm | sigusr1 | sigusr2}

       Output Restart State {=} {off | on}

       Overlay Count {=} Count

       Overwrite {=} {false | no | off | on | true | yes}

       Property PropertyName {=} PropertyValue

       Restart {=} {auto}

       Restart Time {=} Time

       Start Time {=} Start_time

       Synchronize Output

       Shift To Start Time

       Termination Time {=} Final_time

       Timestep Adjustment Interval {=} Nsteps

       Use Dynamic Topology Io

       Use Output Scheduler Timer_name

    end Restart Data Label

### 7.7.5.1. Line Commands

###### Additional Steps

Syntax

  Additional Steps {=} List_of_steps…

Summary

  Additional simulation steps when output should occur.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
List_of_steps | integer… | –

###### Additional Times

Syntax

  Additional Times {=} List_of_times…

Summary

  Additional simulation times when output should occur.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
List_of_times | real… | –

###### At Step

Syntax

  At Step n {increment | interval} {=} m

Summary

  Specify an output interval in terms of the internal iteration step count. The first step specifies the step count at the beginning of this interval and the second step specifies the output frequency to be used within this interval.

Parameter | Value | Default
--- | --- | ---
n | integer | –
Option | {increment | interval} | –
{=} | {= | are | is} | –
m | integer | –

###### At Time

Syntax

  At Time Dt1 {increment | interval} {=} Dt2

Summary

  Specify an output interval in terms of the internal simulation time. The first time specifies the time at the beginning of this time interval and the second time specifies the output frequency to be used within this interval.

Parameter | Value | Default
--- | --- | ---
Dt1 | real | –
Option | {increment | interval} | –
{=} | {= | are | is} | –
Dt2 | real | –

###### At Wall Time

Syntax

  At Wall Time Dt1 {increment | interval} {=} Dt2

Summary

  Write a restart file at a specific wall time since the start of the run. Time string format allows s, m, h, d for seconds, minutes, hours, days

Parameter | Value | Default
--- | --- | ---
Dt1 | string | –
Option | {increment | interval} | –
{=} | {= | are | is} | –
Dt2 | string | –

###### Component Separator Character

Syntax

  Component Separator Character {=} Separator

Summary

  The separator is the single character used to separate the output variable basename (e.g. “stress”) from the suffices (e.g. “xx”, “yy”) when displaying the names of the individual variable components. For example, the default separator is “_”, which results in names similar to “stress_xx”, “stress_yy”, … “stress_zx”. To eliminate the separator, specify an empty string (“”) or NONE.

Parameter | Value | Default
--- | --- | ---
{=} | {= | is} | –
Separator | string | –

###### Cycle Count

Syntax

  Cycle Count {=} Count

Summary

  Specify the number of restart steps which will be written to the restart database before previously written steps are overwritten. For example, if the cycle count is 5 and restart is written every 0.1 seconds, the restart system will write 0.1, 0.2, 0.3, 0.4, 0.5 to the database. It will then overwrite the first step with data from time 0.6, the second with time 0.7. At time 0.8, the database would contain data at times 0.6, 0.7, 0.8, 0.4, 0.5. Note that time will not necessarily be monotonically increasing on a database that specifies the cycle count.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Count | integer | –

###### Database Name

Syntax

  Database Name {=} StreamName

Summary

  The database containing the input and/or output restart data. If this analysis is being restarted, restart data will be read from this file. If the analysis is writing restart data, the data will be written to this file. It will be overwritten if it exists (after being read if applicable). If the filename begins with the ‘/’ character, it is an absolute path; otherwise, the path to the current directory will be prepended to the name. See also the ‘Input Database’ and ‘Output Database’ commands.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
StreamName | string | –

###### Database Type

Syntax

  Database Type {=} {catalyst | catalyst_exodus | cgns | dof | dof_exodus | exodus | exodusii | exonull | generated | genesis | null | parallel_exodus | textmesh}

Summary

  The database type/format used for the restart file.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
DatabaseTypes | {catalyst | catalyst_exodus | cgns | dof | dof_exodus | exodus | exodusii | exonull | generated | genesis | null | parallel_exodus | textmesh} | –

###### Debug Dump

Syntax

  Debug Dump

Summary

  Specify whether the restart system will write the restart data immediately after reading the restart data if the run is restarting. The output data can be compared with the restart input data to determine whether they match.

###### Decomposition Method

Syntax

  Decomposition Method {=} {block | cyclic | external | geom_kway | hsfc | kway | kway_geom | linear | map | metis_sfc | random | rcb | rib | variable}

Summary

  The decomposition algorithm to be used to partition elements to each processor in a parallel run.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Method | {block | cyclic | external | geom_kway | hsfc | kway | kway_geom | linear | map | metis_sfc | random | rcb | rib | variable} | –

###### Exists

Syntax

  Exists {=} {abort | add_suffix | append | overwrite}

Summary

  Specify the behavior when creating this database and there is an existing file with the same name. The default behavior is “OVERWRITE” which deletes the existing file and creates a new file of the same name. “APPEND” will (if possible) append the new data to the end of the existing file. “ABORT” will print an error message and end the analysis. “ADD_SUFFIX” will add a suffix to the file name and output to that file.

Parameter | Value | Default
--- | --- | ---
{=} | {= | is} | –
Option2 | {abort | add_suffix | append | overwrite} | –

###### File Cycle Count

Syntax

  File Cycle Count {=} Count

Summary

  Each restart dump will be written to a separate file suffixed with A,B, … The count specifies how many separate files are used before the cycle repeats. For example, if “FILE CYCLE COUNT = 3” is specified, the restart dumps would be written to file-A.rs, file-B.rs, file-C.rs, file-A.rs, … The maximum value for the cycle count is 26.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Count | integer | –

###### Flush Interval

Syntax

  Flush Interval {=} Option

Summary

  The minimum time interval (in seconds) at which output will be explicitly flushed to disk. The default is 10 seconds.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Option | integer | 10

###### Input Database Name

Syntax

  Input Database Name {=} StreamName

Summary

  The database containing the input restart data. If this analysis is being restarted, restart data will be read from this file. See also the ‘Database’ and ‘Output Database’ commands.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
StreamName | string | –

###### Optional

Syntax

  Optional

Summary

  The database will be read if it exists, but it is not an error if there is no restart database to read for this region during a restarted analysis.

###### Output Database Name

Syntax

  Output Database Name {=} StreamName

Summary

  The database containing the output restart data. If the analysis is writing restart data, the data will be written to this file. It will be overwritten if it exists. See also the ‘Database’ and ‘Input Database’ commands.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
StreamName | string | –

###### Output On Signal

Syntax

  Output On Signal {=} {sigabrt | sigalrm | sigfpe | sighup | sigill | sigint | sigkill | sigpipe | sigquit | sigsegv | sigterm | sigusr1 | sigusr2}

Summary

  When the specified signal is raised, the output stream associated with this block will be output.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Signals | {sigabrt | sigalrm | sigfpe | sighup | sigill | sigint | sigkill | sigpipe | sigquit | sigsegv | sigterm | sigusr1 | sigusr2} | –

###### Output Restart State

Syntax

  Output Restart State {=} {off | on}

Summary

  Outputs the restarted state to the new restarted results file

Description

  NOTE: This command must be placed at the Sierra scope of the input file. Allows the analyst to visualize the restarted state for debugging

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Option | {off | on} | –

###### Overlay Count

Syntax

  Overlay Count {=} Count

Summary

  Specify the number of restart outputs which will be overlaid on top of the last written step. For example, if restarts are being output every 0.1 seconds and the overlay count is specified as 2, then restart will write times 0.1 to step 1 of the database. It will then write 0.2 and 0.3 also to step 1. It will then increment the database step and write 0.4 to step 2; overlay 0.5 and 0.6 on step 2… At the end of the analysis, assuming it runs to completion, the database would have times 0.3, 0.6, 0.9, … However, if there were a problem during the analysis, the last step on the database would contain an intermediate step.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Count | integer | –

###### Overwrite

Syntax

  Overwrite {=} {false | no | off | on | true | yes}

Summary

  (DEPRECATED, Use EXISTS) Specify whether the restart database should be overwritten if it exists. The default behavior is to overwrite unless this command is specified in the restart block and either off, false, or no is specified.

Parameter | Value | Default
--- | --- | ---
{=} | {= | is} | –
Option2 | {false | no | off | on | true | yes} | –

###### Property

Syntax

  Property PropertyName {=} PropertyValue

Summary

  Define a database property named “PropertyName” with the value “PropertyValue”. If PropertyValue consists of all digits, it will define an integer property. If PropertyValue is “true” or “yes” or “false” or “no”, it will define a logical property; otherwise it will define a string property. If PropertyName consists of multiple strings, they will be concatenated together with “_” separating the individual words. Supported properties are typically database dependent; Current properties are:

  - COMPRESSION_LEVEL = [0..9]

  - COMPRESSION_SHUFFLE = true|false|on|off

  - FILE_TYPE = netcdf4 (forces use of netcdf-4 hdf5-based file)

  - INTEGER_SIZE_DB = 4|8

  - INTEGER_SIZE_API = 4|8

  - LOGGING = true|false|on|off

  - MAX_NAME_LENGTH = value

Parameter | Value | Default
--- | --- | ---
PropertyName | string | –
{=} | {= | are | is} | –
PropertyValue | string | –

###### Restart

Syntax

  Restart {=} {auto}

Summary

  Specify automatic restart file read.

Description

  NOTE: This command must be placed at the Sierra scope of the input file.

  Specify that the analysis should be restarted from the last common time on all restart databases for each Region in the analysis. In addition to this line command, each Region in the analysis (strictly, only the region(s) that will be restarted) must have a restart block specifying the database to read the restart state data.

  By default, use of this command will not cause output files (e.g., results, history, heartbeat, restart) to be overwritten. Instead output files will be written with the same basename and the suffix `-s000*`. Common visualization packages are written to handle this file organization gracefully in order for the user to view all results seamlessly.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
{auto} | {auto | automatic} | –

###### Restart Time

Syntax

  Restart Time {=} Time

Summary

  Specify restart file read at a specified time.

Description

  NOTE: This command must be placed at the Sierra scope of the input file.

  Specify the time that the analysis will be restarted. In addition to this line command, each Region in the analysis (strictly, only the region(s) that will be restarted) must have a restart block specifying the database to read the restart state data. The restart ‘time’ must be greater than zero and less than or equal to the termination time.

  By default, use of this command will cause previous output files (e.g., results, history, heartbeat, restart) to be overwritten. If this command is chosen, the onus is placed on the user to ensure that previous output files are not overwritten.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Time | real | –

###### Start Time

Syntax

  Start Time {=} Start_time

Summary

  Specify the time to start outputting results from this output request block. This time overrides all ‘at time’ and ‘at step’ specifications.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Start_time | real | –

###### Synchronize Output

Syntax

  Synchronize Output

Summary

  In an analysis with multiple regions, it is sometimes desirable to synchronize the output of results data between the regions. This can be done by adding the SYNCHRONIZE OUTPUT command line to the results output block. If a results block has this set, then it will write output whenever a previous region writes output. The ordering of regions is based on the order in the input file, algorithmic considerations, or by solution control specifications.

  Although the USE OUTPUT SCHEDULER command line can also synchronize output between regions, the SYNCHRONIZE OUTPUT command line will synchronize the output with regions where the output frequency is not under the direct control of the Sierra IO system. Examples of this are typically coupled applications where one or more of the codes are not Sierra-based applications such as Alegra and CTH. A results block with SYNCHRONIZE OUTPUT specified will also synchronize its output with the output of the external code.

  The SYNCHRONIZE OUTPUT command can be used with other output scheduling commands such as time-based or step-based output specifications.

###### Shift To Start Time

Syntax

  Shift To Start Time

Summary

  The shift to start time option allows a user to shift the restart time to the start time of the current region. An example use case would be if a restart time of 0.5 is specified, but the user would like to start the simulation at time 1.0.

###### Termination Time

Syntax

  Termination Time {=} Final_time

Summary

  Specify the time to stop outputting results from this output request block.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Final_time | real | –

###### Timestep Adjustment Interval

Syntax

  Timestep Adjustment Interval {=} Nsteps

Summary

  Specify the number of steps to ‘look ahead’ and adjust the timestep to ensure that the specified output times or simulation end time will be hit ‘exactly’.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Nsteps | integer | –

###### Use Dynamic Topology Io

Syntax

  Use Dynamic Topology Io

Summary

  Specify that the app use IO for dynamic topology modifications where the output files are stored in a single database. Legacy file format for dynamically changing topology results in the creation of multiple files for each output on a mesh modification. This option leverages the ability of netCDF to create mesh groups within a single database and concatenate all mesh files into one. The names of each mesh group are of the form IOSS_MESH_GROUP-??? where ??? is the 1-based output index 1, 2, …, 10, …., 100, … Please note that netCDF has a current limit of 65,536 groups

###### Use Output Scheduler

Syntax

  Use Output Scheduler Timer_name

Summary

  Associates a predefined output scheduler with this output block (results, restart, heartbeat, or history).

Parameter | Value | Default
--- | --- | ---
Timer_name | string | –

## 7.7.6. Results Output

Scope

  Average Region, Fuego Region, Input_Output Region, Particle Region

Summary

  Describes the location and type of the output stream used for outputting results for the enclosing region.

    begin Results Output Label

       Additional Steps {=} List_of_steps...

       Additional Times {=} List_of_times...

       At Step n {increment | interval} {=} m

       At Time Dt1 {increment | interval} {=} Dt2

       Auto Output {all | element | global | nodal} User Defined Variables [ In UserOutputResultsList...  ]

       Auto Output {all | element | global | nodal} Variables

       Component Separator Character {=} Separator

       Database Name {=} StreamName

       Database Type {=} {catalyst | catalyst_exodus | cgns | dof | dof_exodus | exodus | exodusii | exonull | generated | genesis | null | parallel_exodus | textmesh}

       Edge VariableList...

       Element VariableList...

       Enable Large Ids

       Exclude {=} [ ElementBlockList...  ]

       Exists {=} {abort | add_suffix | append | overwrite}

       Face VariableList...

       Flush Interval {=} Option

       Global VariableList...

       Include {=} [ ElementBlockList...  ]

       Nodal VariableList...

       Node VariableList...

       Nodeset VariableList...

       Output Mesh {=} {exposed surface | refined | unrefined}

       Output On Signal {=} {sigabrt | sigalrm | sigfpe | sighup | sigill | sigint | sigkill | sigpipe | sigquit | sigsegv | sigterm | sigusr1 | sigusr2}

       Overwrite {=} {false | no | off | on | true | yes}

       Property PropertyName {=} PropertyValue

       Sideset VariableList...

       Start Time {=} Start_time

       Surface VariableList...

       Synchronize Output

       Termination Time {=} Final_time

       Timeseries Name {=} filename

       Timestep Adjustment Interval {=} Nsteps

       Title

       Use Dynamic Topology Io

       Use Output Scheduler Timer_name

       begin Catalyst Label
       end

    end Results Output Label

### 7.7.6.1. Line Commands

###### Additional Steps

Syntax

  Additional Steps {=} List_of_steps…

Summary

  Additional simulation steps when output should occur.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
List_of_steps | integer… | –

###### Additional Times

Syntax

  Additional Times {=} List_of_times…

Summary

  Additional simulation times when output should occur.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
List_of_times | real… | –

###### At Step

Syntax

  At Step n {increment | interval} {=} m

Summary

  Specify an output interval in terms of the internal iteration step count. The first step specifies the step count at the beginning of this interval and the second step specifies the output frequency to be used within this interval.

Parameter | Value | Default
--- | --- | ---
n | integer | –
Option | {increment | interval} | –
{=} | {= | are | is} | –
m | integer | –

###### At Time

Syntax

  At Time Dt1 {increment | interval} {=} Dt2

Summary

  Specify an output interval in terms of the internal simulation time. The first time specifies the time at the beginning of this time interval and the second time specifies the output frequency to be used within this interval.

Parameter | Value | Default
--- | --- | ---
Dt1 | real | –
Option | {increment | interval} | –
{=} | {= | are | is} | –
Dt2 | real | –

###### Auto Output

Syntax

  Auto Output {all | element | global | nodal} User Defined Variables [ In UserOutputResultsList… ]

Summary

  Allows users to automatically output all user output defined variables for the type requested.

Parameter | Value | Default
--- | --- | ---
auto_output_type_3 | {all | element | global | nodal} | –

###### Auto Output

Syntax

  Auto Output {all | element | global | nodal} Variables

Summary

  Allows users to automatically output all user output defined variables for the type requested.

Parameter | Value | Default
--- | --- | ---
auto_output_type_3 | {all | element | global | nodal} | –

###### Component Separator Character

Syntax

  Component Separator Character {=} Separator

Summary

  The separator is the single character used to separate the output variable basename (e.g. “stress”) from the suffices (e.g. “xx”, “yy”) when displaying the names of the individual variable components. For example, the default separator is “_”, which results in names similar to “stress_xx”, “stress_yy”, … “stress_zx”. To eliminate the separator, specify an empty string (“”) or NONE.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Separator | string | –

###### Database Name

Syntax

  Database Name {=} StreamName

Summary

  The base name of the database containing the output results. If the filename begins with the ‘/’ character, it is an absolute path; otherwise, the path to the current directory will be prepended to the name. If this line is omitted, then a filename will be created from the basename of the input file with a “.e” suffix appended.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
StreamName | string | –

###### Database Type

Syntax

  Database Type {=} {catalyst | catalyst_exodus | cgns | dof | dof_exodus | exodus | exodusii | exonull | generated | genesis | null | parallel_exodus | textmesh}

Summary

  The database type/format to be used for the output results.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
DatabaseType | {catalyst | catalyst_exodus | cgns | dof | dof_exodus | exodus | exodusii | exonull | generated | genesis | null | parallel_exodus | textmesh} | –

###### Edge

Syntax

  Edge VariableList…

Summary

  Define the variables that should be written to the results database. If “variable” is entered, then its name will be used on the output database. If “variable as db_name” is entered, then “db_name” will be the name used on the database for the internal variable “variable”. Multiple “variable” or “variable as db_name” entries are allowed on the same line. The entities that this variable are written to can also be limited or specified with “exclude list_of_entities” or “include list_of_entities”. Edge variables are not supported for all database types.

Parameter | Value | Default
--- | --- | ---
VariableList | string… | –

###### Element

Syntax

  Element VariableList…

Summary

  Define the variables that should be written to the results database. If “variable” is entered, then its name will be used on the output database. If “variable as db_name” is entered, then “db_name” will be the name used on the database for the internal variable “variable”. Multiple “variable” or “variable as db_name” entries are allowed on the same line. The entities that this variable are written to can also be limited or specified with “exclude list_of_entities” or “include list_of_entities”

Parameter | Value | Default
--- | --- | ---
VariableList | string… | –

###### Enable Large Ids

Syntax

  Enable Large Ids

Summary

  Enable 64 bit entity IDs for output

###### Exclude

Syntax

  Exclude {=} [ ElementBlockList… ]

Summary

  Specify that the results file will only contain a subset of the element blocks in the analysis model. The element_block_list lists only the blocks which will not be output to the results database.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –

###### Exists

Syntax

  Exists {=} {abort | add_suffix | append | overwrite}

Summary

  Specify the behavior when creating this database and there is an existing file with the same name. The default behavior is “OVERWRITE” which deletes the existing file and creates a new file of the same name. “APPEND” will (if possible) append the new data to the end of the existing file. “ABORT” will print an error message and end the analysis. “ADD_SUFFIX” will add a -s???? suffix where the ???? is replaced by a sequential number starting at 0002.

Parameter | Value | Default
--- | --- | ---
{=} | {= | is} | –
Option2 | {abort | add_suffix | append | overwrite} | –

###### Face

Syntax

  Face VariableList…

Summary

  Define the variables that should be written to the results database. If “variable” is entered, then its name will be used on the output database. If “variable as db_name” is entered, then “db_name” will be the name used on the database for the internal variable “variable”. Multiple “variable” or “variable as db_name” entries are allowed on the same line. The entities that this variable are written to can also be limited or specified with “exclude list_of_entities” or “include list_of_entities”. Face variables are not supported for all database types.

Parameter | Value | Default
--- | --- | ---
VariableList | string… | –

###### Flush Interval

Syntax

  Flush Interval {=} Option

Summary

  The minimum time interval (in seconds) at which output will be explicitly flushed to disk. The default is 10 seconds.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Option | integer | 10

###### Global

Syntax

  Global VariableList…

Summary

  Define the global variables that should be written to the results database. If “variable” is entered, then its name will be used on the output database. If “variable as db_name” is entered, then “db_name” will be the name used on the database for the internal variable “variable”. Multiple “variable” or “variable as db_name” entries are allowed on the same line.

Parameter | Value | Default
--- | --- | ---
VariableList | string… | –

###### Include

Syntax

  Include {=} [ ElementBlockList… ]

Summary

  Specify that the results file will only contain a subset of the element blocks in the analysis model. The element_block_list lists only the blocks which will be output to the results database.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –

###### Nodal

Syntax

  Nodal VariableList…

Summary

  Define the nodal variables that should be written to the results database. If “variable” is entered, then its name will be used on the output database. If “variable as db_name” is entered, then “db_name” will be the name used on the database for the internal variable “variable”. Multiple “variable” or “variable as db_name” entries are allowed on the same line.

Parameter | Value | Default
--- | --- | ---
VariableList | string… | –

###### Node

Syntax

  Node VariableList…

Summary

  Define the nodal variables that should be written to the results database. If “variable” is entered, then its name will be used on the output database. If “variable as db_name” is entered, then “db_name” will be the name used on the database for the internal variable “variable”. Multiple “variable” or “variable as db_name” entries are allowed on the same line.

Parameter | Value | Default
--- | --- | ---
VariableList | string… | –

###### Nodeset

Syntax

  Nodeset VariableList…

Summary

  Define the variables that should be written to the results database. If “variable” is entered, then its name will be used on the output database. If “variable as db_name” is entered, then “db_name” will be the name used on the database for the internal variable “variable”. Multiple “variable” or “variable as db_name” entries are allowed on the same line. The entities that this variable are written to can also be limited or specified with “exclude list_of_entities” or “include list_of_entities”. Nodeset variables are not supported for all database types.

Parameter | Value | Default
--- | --- | ---
VariableList | string… | –

###### Output Mesh

Syntax

  Output Mesh {=} {exposed surface | refined | unrefined}

Summary

  Use this command to turn on “unrefined” as the output mesh. The default behavior is “refined”, in which field variables are output on the current mesh, which may have been refined (either uniformly or adaptively) or had its topology altered in some way (e.g., dynamic load balancing) with respect to the original mesh read from the input file. By specifying “Output Mesh = unrefined”, all output variables are output only on the original mesh objects read from the input file.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
OutputMesh | {exposed surface | refined | unrefined} | –

###### Output On Signal

Syntax

  Output On Signal {=} {sigabrt | sigalrm | sigfpe | sighup | sigill | sigint | sigkill | sigpipe | sigquit | sigsegv | sigterm | sigusr1 | sigusr2}

Summary

  When the specified signal is raised, the output stream associated with this block will be output.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Signals | {sigabrt | sigalrm | sigfpe | sighup | sigill | sigint | sigkill | sigpipe | sigquit | sigsegv | sigterm | sigusr1 | sigusr2} | –

###### Overwrite

Syntax

  Overwrite {=} {false | no | off | on | true | yes}

Summary

  (DEPRECATED, Use EXISTS) Specify whether the database should be overwritten if it exists. The default behavior is to overwrite unless this command is specified in the output block and either off, false, or no is specified.

Parameter | Value | Default
--- | --- | ---
{=} | {= | is} | –
Option2 | {false | no | off | on | true | yes} | –

###### Property

Syntax

  Property PropertyName {=} PropertyValue

Summary

  Define a database property named “PropertyName” with the value “PropertyValue”. If PropertyValue consists of all digits, it will define an integer property. If PropertyValue is “true” or “yes” or “false” or “no”, it will define a logical property; otherwise it will define a string property. Supported properties are typically database dependent; Current properties are:

  - COMPRESSION_LEVEL = [0..9] (off)

  - COMPRESSION_SHUFFLE = true|false|on|off (off)

  - FILE_TYPE = netcdf4 (forces use of netcdf-4 hdf5-based file) (netcdf3)

  - INTEGER_SIZE_DB = 4|8 (4)

  - INTEGER_SIZE_API = 4|8 (4)

  - REAL_SIZE_DB = 4|8 (8 is default)

  - LOGGING = true|false|on|off (off)

  - MAX_NAME_LENGTH = value (32)

Parameter | Value | Default
--- | --- | ---
PropertyName | string | –
{=} | {= | are | is} | –
PropertyValue | string | –

###### Sideset

Syntax

  Sideset VariableList…

Summary

  Define the variables that should be written to the results database. If “variable” is entered, then its name will be used on the output database. If “variable as db_name” is entered, then “db_name” will be the name used on the database for the internal variable “variable”. Multiple “variable” or “variable as db_name” entries are allowed on the same line. The entities that this variable are written to can also be limited or specified with “exclude list_of_entities” or “include list_of_entities”. Face variables are not supported for all database types.

Parameter | Value | Default
--- | --- | ---
VariableList | string… | –

###### Start Time

Syntax

  Start Time {=} Start_time

Summary

  Specify the time to start outputting results from this output request block. This time overrides all ‘at time’ and ‘at step’ specifications.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Start_time | real | –

###### Surface

Syntax

  Surface VariableList…

Summary

  Define the variables that should be written to the results database. If “variable” is entered, then its name will be used on the output database. If “variable as db_name” is entered, then “db_name” will be the name used on the database for the internal variable “variable”. Multiple “variable” or “variable as db_name” entries are allowed on the same line. The entities that this variable are written to can also be limited or specified with “exclude list_of_entities” or “include list_of_entities”. Face variables are not supported for all database types.

Parameter | Value | Default
--- | --- | ---
VariableList | string… | –

###### Synchronize Output

Syntax

  Synchronize Output

Summary

  In an analysis with multiple regions, it is sometimes desirable to synchronize the output of results data between the regions. This can be done by adding the SYNCHRONIZE OUTPUT command line to the results output block. If a results block has this set, then it will write output whenever a previous region writes output. The ordering of regions is based on the order in the input file, algorithmic considerations, or by solution control specifications.

  Although the USE OUTPUT SCHEDULER command line can also synchronize output between regions, the SYNCHRONIZE OUTPUT command line will synchronize the output with regions where the output frequency is not under the direct control of the Sierra IO system. Examples of this are typically coupled applications where one or more of the codes are not Sierra-based applications such as Alegra and CTH. A results block with SYNCHRONIZE OUTPUT specified will also synchronize its output with the output of the external code.

  The SYNCHRONIZE OUTPUT command can be used with other output scheduling commands such as time-based or step-based output specifications.

###### Termination Time

Syntax

  Termination Time {=} Final_time

Summary

  Specify the time to stop outputting results from this output request block.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Final_time | real | –

###### Timeseries Name

Syntax

  Timeseries Name {=} filename

Summary

  Optionally specify a filename for a timeseries file that outputs the root database filename in the order that they are written. This is useful when running on large numbers of processors with many mesh-mods that cause simple disk operations to hang.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
filename | string | –

###### Timestep Adjustment Interval

Syntax

  Timestep Adjustment Interval {=} Nsteps

Summary

  Specify the number of steps to ‘look ahead’ and adjust the timestep to ensure that the specified output times or simulation end time will be hit ‘exactly’.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Nsteps | integer | –

###### Title

Syntax

  Title

Summary

  Specify the title to be used for this specific output block.

###### Use Dynamic Topology Io

Syntax

  Use Dynamic Topology Io

Summary

  Specify that the app use IO for dynamic topology modifications where the output files are stored in a single database. Legacy file format for dynamically changing topology results in the creation of multiple files for each output on a mesh modification. This option leverages the ability of netCDF to create mesh groups within a single database and concatenate all mesh files into one. The names of each mesh group are of the form IOSS_MESH_GROUP-??? where ??? is the 1-based output index 1, 2, …, 10, …., 100, … Please note that netCDF has a current limit of 65,536 groups

###### Use Output Scheduler

Syntax

  Use Output Scheduler Timer_name

Summary

  Associates a predefined output scheduler with this output block (results, restart, heartbeat, or history).

Parameter | Value | Default
--- | --- | ---
Timer_name | string | –

## 7.7.7. Solid Object

Scope

  Fuego Region

Summary

  Contains the commands needed to create a solid object

    begin Solid Object Objectname

       Cylinder Base {=} Param21 Param22 Param23 Top {=} Param51 Param52 Param53 Radius {=} Param8

       Rectangle Center {=} Param21 Param22 Param23 Xyz {=} Param51 Param52 Param53

       Sphere Center {=} Param21 Param22 Param23 Radius {=} Param5

    end Solid Object Objectname

### 7.7.7.1. Line Commands

###### Cylinder

Syntax

  Cylinder Base {=} Param21 Param22 Param23 Top {=} Param51 Param52 Param53 Radius {=} Param8

Summary

  Specify cylinder as interface surface, with given radius and two endpoints of axis p1(base) and p2(top). The length of the cylinder is norm(p2 - p1).

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Param2 | real1 real2 real3 | –
{=} | {= | are | is} | –
Param5 | real1 real2 real3 | –
{=} | {= | are | is} | –
Param8 | real | –

###### Rectangle

Syntax

  Rectangle Center {=} Param21 Param22 Param23 Xyz {=} Param51 Param52 Param53

Summary

  Specify rectangle as interface surface, with given center and x,y,z sizes.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Param2 | real1 real2 real3 | –
{=} | {= | are | is} | –
Param5 | real1 real2 real3 | –

###### Sphere

Syntax

  Sphere Center {=} Param21 Param22 Param23 Radius {=} Param5

Summary

  Specify sphere as interface surface with given center and radius.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Param2 | real1 real2 real3 | –
{=} | {= | are | is} | –
Param5 | real | –

## 7.7.8. Virtual Thermocouple Model On Block

Scope

  Fuego Region

Summary

  Activate the virtual thermocouple model on the requested mesh block

Description

  The virtual thermocouple model assumes one-way coupling between the fluid and the thermocouple. The thermocouple is assumed to be small enough that it does not influence the fluid behavior in any way.

  For simulations without a PMR solve the radiative terms of the thermocouple equation are neglected.

    begin Virtual Thermocouple Model On Block BlockName

       Compute Steady Solution

       Density {=} Value

       Diameter {=} Value

       Emissivity {=} Value

       Heat Capacity {=} Value

       Initial Temperature {=} Value

       Length {=} Value

       Orientation {=} Lx Ly [ Lz  ]

    end Virtual Thermocouple Model On Block BlockName

### 7.7.8.1. Line Commands

###### Compute Steady Solution

Syntax

  Compute Steady Solution

Summary

  Compute the steady-state temperature for the thermocouple given the current FUEGO/SRYINX solutions. By default, the thermocouple temperature will be updated in a time-accurate manner.

###### Density

Syntax

  Density {=} Value

Summary

  Specify the density of the thermocouple

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Value | real | –

###### Diameter

Syntax

  Diameter {=} Value

Summary

  Specify the diameter of the thermocouple (assumed to be a cylinder)

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Value | real | –

###### Emissivity

Syntax

  Emissivity {=} Value

Summary

  Specify the emissivity of the thermocouple

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Value | real | –

###### Heat Capacity

Syntax

  Heat Capacity {=} Value

Summary

  Specify the heat capacity of the thermocouple

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Value | real | –

###### Initial Temperature

Syntax

  Initial Temperature {=} Value

Summary

  Specify the initial temperature of the thermocouple

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Value | real | –

###### Length

Syntax

  Length {=} Value

Summary

  Specify the length of the thermocouple (assumed to be a cylinder)

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Value | real | –

###### Orientation

Syntax

  Orientation {=} Lx Ly [ Lz ]

Summary

  Specify the spatial orientation vector of the thermocouple

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Lx | real | –
Ly | real | –

## 7.7.9. Solution Options

Scope

  Average Region, Fuego Region

Summary

  Specify information regarding the governing equations to be solved.

    begin Solution Options OptionsName

       Activate Acoustic Compressibility Algorithm

       Activate Equation {conserved_enthalpy | continuity | edc_product | enthalpy | mixture_fraction | nuclei | progress_variable | scalar_variance | second_mixture_fraction | solid_volume_fraction | soot | species | temperature | turbulent_dissipation | turbulent_frequency | turbulent_helmholtz_function | turbulent_kinetic_energy | turbulent_v2 | volume_of_fluid | x_momentum | x_solid_momentum | y_momentum | y_solid_momentum | z_momentum | z_solid_momentum}

       Activate Full Surface Cvfem Gradient Operator For Muscl Scheme

       Activate Lighthill Tensor Postprocessing

       Activate Species Enthalpy Calculations

       Activate Viscous Dissipation Source Term

       Compute Steady Solution Using Pseudo Transient Method

       Coordinate System {=} {2d | 3d | xaxi | yaxi}

       First Order Upwind Factor {=} Value [ For Equation {conserved_enthalpy | continuity | edc_product | enthalpy | mixture_fraction | nuclei | progress_variable | scalar_variance | second_mixture_fraction | solid_volume_fraction | soot | species | temperature | turbulent_dissipation | turbulent_frequency | turbulent_helmholtz_function | turbulent_kinetic_energy | turbulent_v2 | volume_of_fluid | x_momentum | x_solid_momentum | y_momentum | y_solid_momentum | z_momentum | z_solid_momentum}  ]

       Fix Pressure To FixedPressure At A Single Node

       Hybrid Upwind Factor {=} Value [ For Equation {conserved_enthalpy | continuity | edc_product | enthalpy | mixture_fraction | nuclei | progress_variable | scalar_variance | second_mixture_fraction | solid_volume_fraction | soot | species | temperature | turbulent_dissipation | turbulent_frequency | turbulent_helmholtz_function | turbulent_kinetic_energy | turbulent_v2 | volume_of_fluid | x_momentum | x_solid_momentum | y_momentum | y_solid_momentum | z_momentum | z_solid_momentum}  ]

       Hybrid Upwind Method {=} {blending | tanh} [ For Equation {conserved_enthalpy | continuity | edc_product | enthalpy | mixture_fraction | nuclei | progress_variable | scalar_variance | second_mixture_fraction | solid_volume_fraction | soot | species | temperature | turbulent_dissipation | turbulent_frequency | turbulent_helmholtz_function | turbulent_kinetic_energy | turbulent_v2 | volume_of_fluid | x_momentum | x_solid_momentum | y_momentum | y_solid_momentum | z_momentum | z_solid_momentum}  ]

       Hybrid Upwind Shift {=} Value [ For Equation {conserved_enthalpy | continuity | edc_product | enthalpy | mixture_fraction | nuclei | progress_variable | scalar_variance | second_mixture_fraction | solid_volume_fraction | soot | species | temperature | turbulent_dissipation | turbulent_frequency | turbulent_helmholtz_function | turbulent_kinetic_energy | turbulent_v2 | volume_of_fluid | x_momentum | x_solid_momentum | y_momentum | y_solid_momentum | z_momentum | z_solid_momentum}  ]

       Hybrid Upwind Width {=} Value [ For Equation {conserved_enthalpy | continuity | edc_product | enthalpy | mixture_fraction | nuclei | progress_variable | scalar_variance | second_mixture_fraction | solid_volume_fraction | soot | species | temperature | turbulent_dissipation | turbulent_frequency | turbulent_helmholtz_function | turbulent_kinetic_energy | turbulent_v2 | volume_of_fluid | x_momentum | x_solid_momentum | y_momentum | y_solid_momentum | z_momentum | z_solid_momentum}  ]

       Include Continuity Residual Term [ With Diagnostics  ]

       Lighthill Tensor Smoothing Iterations {=} Number

       Maximum Number Of Continuity_Momentum Nonlinear Iterations {=} Number

       Maximum Number Of Energy_Species Nonlinear Iterations {=} Number

       Maximum Number Of Gas_Solid_Momentum Nonlinear Iterations {=} Number

       Maximum Number Of Kepsilon Nonlinear Iterations {=} Number

       Maximum Number Of Komega Nonlinear Iterations {=} Number

       Maximum Number Of Ksgs Nonlinear Iterations {=} Number

       Maximum Number Of Mixture Fraction Nonlinear Iterations {=} Number

       Maximum Number Of Nonlinear Iterations {=} Number

       Maximum Number Of Solid Phase Nonlinear Iterations {=} Number

       Maximum Number Of Soot Nuclei Nonlinear Iterations {=} Number

       Maximum Number Of Species Nonlinear Iterations {=} Number

       Maximum Number Of Species_Product Nonlinear Iterations {=} Number

       Maximum Number Of V2F Nonlinear Iterations {=} Number

       Maximum Wall Time {=} WallTime Hours

       Minimum Number Of Nonlinear Iterations {=} Number

       Nonlinear Residual Norm Tolerance {=} Tolerance [ For Equation {conserved_enthalpy | continuity | edc_product | enthalpy | mixture_fraction | nuclei | progress_variable | scalar_variance | second_mixture_fraction | solid_volume_fraction | soot | species | temperature | turbulent_dissipation | turbulent_frequency | turbulent_helmholtz_function | turbulent_kinetic_energy | turbulent_v2 | volume_of_fluid | x_momentum | x_solid_momentum | y_momentum | y_solid_momentum | z_momentum | z_solid_momentum}  ]

       Nonlinear Stabilization Method {=} {commutation_error | none | pointwise_residual_error} [ For Equation {conserved_enthalpy | continuity | edc_product | enthalpy | mixture_fraction | nuclei | progress_variable | scalar_variance | second_mixture_fraction | solid_volume_fraction | soot | species | temperature | turbulent_dissipation | turbulent_frequency | turbulent_helmholtz_function | turbulent_kinetic_energy | turbulent_v2 | volume_of_fluid | x_momentum | x_solid_momentum | y_momentum | y_solid_momentum | z_momentum | z_solid_momentum}  ]

       Omit Density Time Derivative In Continuity Equation [ For OmitSteps Steps And Blend In Over BlendSteps Steps  ]

       Output Nonlinear Residual Field For Equation {conserved_enthalpy | continuity | edc_product | enthalpy | mixture_fraction | nuclei | progress_variable | scalar_variance | second_mixture_fraction | solid_volume_fraction | soot | species | temperature | turbulent_dissipation | turbulent_frequency | turbulent_helmholtz_function | turbulent_kinetic_energy | turbulent_v2 | volume_of_fluid | x_momentum | x_solid_momentum | y_momentum | y_solid_momentum | z_momentum | z_solid_momentum} As ResName [ On Output Block BlockName  ]

       Periodic Constant Momentum Body Source Term {=} ConstSrc1 ConstSrc2 ConstSrc3

       Progress Variable Source Evaluation Time {=} {latest | presolve}

       Projection Method {=} {fourth_order | second_order | stabilized | zeroth_order} Smoothing [ With {characteristic | momentum | timestep} Scaling  ]

       Randomize Pressure

       Skip Pressure Update If Continuity Solve Fails

       Source Term Function {=} FuncStr For Equation {conserved_enthalpy | continuity | edc_product | enthalpy | mixture_fraction | nuclei | progress_variable | scalar_variance | second_mixture_fraction | solid_volume_fraction | soot | species | temperature | turbulent_dissipation | turbulent_frequency | turbulent_helmholtz_function | turbulent_kinetic_energy | turbulent_v2 | volume_of_fluid | x_momentum | x_solid_momentum | y_momentum | y_solid_momentum | z_momentum | z_solid_momentum} [ VariableName  ]

       Source Term Subroutine {=} Subroutine For Equation {conserved_enthalpy | continuity | edc_product | enthalpy | mixture_fraction | nuclei | progress_variable | scalar_variance | second_mixture_fraction | solid_volume_fraction | soot | species | temperature | turbulent_dissipation | turbulent_frequency | turbulent_helmholtz_function | turbulent_kinetic_energy | turbulent_v2 | volume_of_fluid | x_momentum | x_solid_momentum | y_momentum | y_solid_momentum | z_momentum | z_solid_momentum} [ VariableName  ]

       Stop Simulation If Peak Velocity Exceeds MaxVel

       Under Relax {conserved_enthalpy | continuity | edc_product | enthalpy | mixture_fraction | nuclei | progress_variable | scalar_variance | second_mixture_fraction | solid_volume_fraction | soot | species | temperature | turbulent_dissipation | turbulent_frequency | turbulent_helmholtz_function | turbulent_kinetic_energy | turbulent_v2 | volume_of_fluid | x_momentum | x_solid_momentum | y_momentum | y_solid_momentum | z_momentum | z_solid_momentum} By Urf [ With Implicit Term  ]

       Under Relax Momentum By Urf

       Under Relax Pressure By Urf

       Under Relax Solid_Momentum By Urf

       Under Relax Temperature_Extraction By Urf

       Upwind Limiter {=} {minmod | none | superbee | van_albada | van_leer} [ For Equation {conserved_enthalpy | continuity | edc_product | enthalpy | mixture_fraction | nuclei | progress_variable | scalar_variance | second_mixture_fraction | solid_volume_fraction | soot | species | temperature | turbulent_dissipation | turbulent_frequency | turbulent_helmholtz_function | turbulent_kinetic_energy | turbulent_v2 | volume_of_fluid | x_momentum | x_solid_momentum | y_momentum | y_solid_momentum | z_momentum | z_solid_momentum}  ]

       Upwind Method {=} {lps | muscl | upw} [ For Equation {conserved_enthalpy | continuity | edc_product | enthalpy | mixture_fraction | nuclei | progress_variable | scalar_variance | second_mixture_fraction | solid_volume_fraction | soot | species | temperature | turbulent_dissipation | turbulent_frequency | turbulent_helmholtz_function | turbulent_kinetic_energy | turbulent_v2 | volume_of_fluid | x_momentum | x_solid_momentum | y_momentum | y_solid_momentum | z_momentum | z_solid_momentum}  ]

       Use Equation Solver SolverName For Equation {conserved_enthalpy | continuity | edc_product | enthalpy | mixture_fraction | nuclei | progress_variable | scalar_variance | second_mixture_fraction | solid_volume_fraction | soot | species | temperature | turbulent_dissipation | turbulent_frequency | turbulent_helmholtz_function | turbulent_kinetic_energy | turbulent_v2 | volume_of_fluid | x_momentum | x_solid_momentum | y_momentum | y_solid_momentum | z_momentum | z_solid_momentum}

       Use External Continuity Source

       Use External Energy Source

       Use External Mixture_Fraction Source

       Use External Momentum Source

       Use External Soot_Mass_Fraction Source

       Use External Species Source

       Use Lumped Velocity Density Interpolation

       Use Radiation Source From External Region [ Using Classic Linearization  ]

       Use Shifted Density Iteration

       Use Skew Symmetric Central Operator [ For Equation {conserved_enthalpy | continuity | edc_product | enthalpy | mixture_fraction | nuclei | progress_variable | scalar_variance | second_mixture_fraction | solid_volume_fraction | soot | species | temperature | turbulent_dissipation | turbulent_frequency | turbulent_helmholtz_function | turbulent_kinetic_energy | turbulent_v2 | volume_of_fluid | x_momentum | x_solid_momentum | y_momentum | y_solid_momentum | z_momentum | z_solid_momentum}  ]

       begin Acoustic Transfer Output DefinitionName
       end

       begin Beam Radiation Boundary Specification DefinitionName
       end

       begin Buoyancy Model Specification BuoyModelName
       end

       begin Edc Model Specification EdcSpecName
       end

       begin Mesh Motion Specification DefinitionName
       end

       begin Multiphase Model Specification DefinitionName
       end

       begin Point Source DefinitionName
       end

       begin Rad Transport Spectral Model Specification DefinitionName
       end

       begin Radiation Transport Equation Model Specification RadModelName
       end

       begin Time Integration Specification TimeIntSpecName
       end

       begin Turbulence Model Specification TurbSpecName
       end

       begin Vof Model Specification DefinitionName
       end

    end Solution Options OptionsName

### 7.7.9.1. Line Commands

###### Activate Acoustic Compressibility Algorithm

Syntax

  Activate Acoustic Compressibility Algorithm

Summary

  Variable thermodynamic pressure

Description

  This option will allow for closed system pressurization either through heat-up or inflow of fluid.

  The algorithm will add the substantial derivative of pressure, , to the laminar or turbulent enthalpy transport equation and to the laminar temperature transport equation. Additionally, the viscous work term will be added to the turbulent enthalpy equation. An implicit term in the continuity solve is added through the time density derivative. As such, Cantera support is required. The convective terms within the continuity solve are neglected.

  Caveats for this model:

  1. The Cantera material model evaluator must be used.

  2) The initial pressure and any boundary condition pressures must be specified with respect to the datum pressure.

  If a zero datum pressure is specified, then all initial and boundary pressures will be in absolute units. If this is a coupled structural simulation, then the surface traction due to this pressure will need to be counteracted with a load on the “back side” that is equivalent to the ambient pressure in absolute units.

  If a non-zero datum pressure is specified, then all initial and boundary pressures will be in relative units with respect to this datum. Pressure can then be thought of as a gauge pressure with respect to the datum. The “back side” load in structural simulations must be set accordingly. (For example, if the datum is set equal to the external ambient pressure, 1 atm, and the initial pressure is set to zero, then the initial surface traction force due to pressure will be zero and no “back side” load due to the ambient pressure should be specified.)

###### Activate Equation

Syntax

  Activate Equation {conserved_enthalpy | continuity | edc_product | enthalpy | mixture_fraction | nuclei | progress_variable | scalar_variance | second_mixture_fraction | solid_volume_fraction | soot | species | temperature | turbulent_dissipation | turbulent_frequency | turbulent_helmholtz_function | turbulent_kinetic_energy | turbulent_v2 | volume_of_fluid | x_momentum | x_solid_momentum | y_momentum | y_solid_momentum | z_momentum | z_solid_momentum}

Summary

  Activate the specified equation.

Parameter | Value | Default
--- | --- | ---
Equations | {conserved_enthalpy | continuity | edc_product | enthalpy | mixture_fraction | nuclei | progress_variable | scalar_variance | second_mixture_fraction | solid_volume_fraction | soot | species | temperature | turbulent_dissipation | turbulent_frequency | turbulent_helmholtz_function | turbulent_kinetic_energy | turbulent_v2 | volume_of_fluid | x_momentum | x_solid_momentum | y_momentum | y_solid_momentum | z_momentum | z_solid_momentum} | –

###### Activate Full Surface Cvfem Gradient Operator For Muscl Scheme

Syntax

  Activate Full Surface Cvfem Gradient Operator For Muscl Scheme

Summary

  Use full stencil for gradient used in MUSCL convection operator

Description

  The default gradient operator for the MUSCL scheme is the edge-based stencil. This option keeps integration points at the subcontrol surface points.

###### Activate Lighthill Tensor Postprocessing

Syntax

  Activate Lighthill Tensor Postprocessing

Summary

  Postprocesses the nodal divergence of the Lighthill tensor

Description

  This calculates the nodal divergence of the Lighthill tensor, used for acoustic analysis.

###### Activate Species Enthalpy Calculations

Syntax

  Activate Species Enthalpy Calculations

Summary

  Enables calculation of species enthalpy

Description

  This forces the calculation of species enthalpy, needed primarily for coupled Fuego-Aria problems.

###### Activate Viscous Dissipation Source Term

Syntax

  Activate Viscous Dissipation Source Term

Summary

  Add viscous dissipation source term

Description

  For low speed viscous dissipation effects, this source term will provide the viscous work source term in the static enthalpy equation. This source term is a subset of the full acoustically compressible source term option, however, the substantial pressure derivative is omitted.

###### Compute Steady Solution Using Pseudo Transient Method

Syntax

  Compute Steady Solution Using Pseudo Transient Method

Summary

  Compute a steady-state solution using the pseudo-transient method (time march to steady solution).

Description

  The solution will march forward in time until either the stopping time is reached or the steady convergence criterion is met. Convergence to steady state is detected when all equations meet their nonlinear residual norm tolerances after the first nonlinear iteration, since this will only occur as the solution stops changing between time steps. The nonlinear residual norm tolerances should be set small enough to prevent false positives. Also make sure the simulation time is set to be fairly large, to prevent a premature end to the simulation before convergence is achieved.

  If you are using solution control, then you also need to test for a region parameter to stop the simulation. In your `PARAMETERS FOR TRANSIENT` solution control block, add the line (assuming your Fuego region is called `fuego_region`):

      CONVERGED WHEN "fuego_region.REGION_STEADY_STATE == 1"

###### Coordinate System

Syntax

  Coordinate System {=} {2d | 3d | xaxi | yaxi}

Summary

  Specify the coordinate system.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
CoordSys | {2d | 3d | xaxi | yaxi} | 3D

###### First Order Upwind Factor

Syntax

  First Order Upwind Factor {=} Value [ For Equation {conserved_enthalpy | continuity | edc_product | enthalpy | mixture_fraction | nuclei | progress_variable | scalar_variance | second_mixture_fraction | solid_volume_fraction | soot | species | temperature | turbulent_dissipation | turbulent_frequency | turbulent_helmholtz_function | turbulent_kinetic_energy | turbulent_v2 | volume_of_fluid | x_momentum | x_solid_momentum | y_momentum | y_solid_momentum | z_momentum | z_solid_momentum} ]

Summary

  First-order upwind factor,

Description

  This value specifies the explicit upwind blending between pure upwind and the chosen convection operator, e.g., UPW*(firstOrderUpwind) + (1-firstOrderUpwind)*(blendedUpwindCentral).

  where UPW is the pure first order upwind value and blendedUpwindCentral is a blend between the selected upwind method and central difference operator based on the local cell Peclet number (see Hybrid Upwind Factor line command). The value can be a time dependent string function.

  Values for individual equation sets may be set using optional token. Using both (in either order):

  - FIRST ORDER UPWIND FACTOR = String

  - FIRST ORDER UPWIND FACTOR = String FOR EQUATION Equations

  Will result in the particular equation set to specified value while all others set to general value.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Value | “string” | 1.0

###### Fix Pressure To

Syntax

  Fix Pressure To FixedPressure At A Single Node

Summary

  Sets a dirichlet for pressure at a single arbitrary node. This is required for a well posed pressure equation if none of the boundaries specify pressure (e.g. open).

Parameter | Value | Default
--- | --- | ---
FixedPressure | real | 0.0

###### Hybrid Upwind Factor

Syntax

  Hybrid Upwind Factor {=} Value [ For Equation {conserved_enthalpy | continuity | edc_product | enthalpy | mixture_fraction | nuclei | progress_variable | scalar_variance | second_mixture_fraction | solid_volume_fraction | soot | species | temperature | turbulent_dissipation | turbulent_frequency | turbulent_helmholtz_function | turbulent_kinetic_energy | turbulent_v2 | volume_of_fluid | x_momentum | x_solid_momentum | y_momentum | y_solid_momentum | z_momentum | z_solid_momentum} ]

Summary

  Hybrid upwinding factor.

Description

  The upwind schemes are blended with a centered scheme. The HYBRID UPWIND FACTOR is a multiplier against the cell Peclet number used in the switching scheme (see First Order Upwind Factor line command).

  - A HYBRID UPWIND FACTOR = 0.0 results in all centered.

  - A HYBRID UPWIND FACTOR = 1.0 results in default hybrid.

  - A HYBRID UPWIND FACTOR >> 1.0 results in all upwind.

  Values for individual equation sets may be set using optional token. Using both (in either order):

  - HYBRID UPWIND FACTOR = String

  - HYBRID UPWIND FACTOR = String FOR EQUATION Equations

  Will result in the particular equation set to specified value while all others set to general value. The value can be specified as a time dependent string function or a constant.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Value | “string” | 1.0

###### Hybrid Upwind Method

Syntax

  Hybrid Upwind Method {=} {blending | tanh} [ For Equation {conserved_enthalpy | continuity | edc_product | enthalpy | mixture_fraction | nuclei | progress_variable | scalar_variance | second_mixture_fraction | solid_volume_fraction | soot | species | temperature | turbulent_dissipation | turbulent_frequency | turbulent_helmholtz_function | turbulent_kinetic_energy | turbulent_v2 | volume_of_fluid | x_momentum | x_solid_momentum | y_momentum | y_solid_momentum | z_momentum | z_solid_momentum} ]

Summary

  Hybriding method between central and upwind using Peclet number

Description

  BLENDING and TANH approaches are currently supported.

  Function determines the ratio between user-chosen upwind () and central (1-) operators. The need for an upwind operator is affected by cell-Peclet number.

  BLENDING uses HYBRID UPWIND FACTOR () and the function is, .

  TAHH follows hyperbolic tangent profile between and Pe. It uses shift p (HYBRID UPWIND SHIFT) and width w (HYBRID UPWIND WIDTH) parameters as, . Tanh is centered () when Peclet number is at the shifting factor p. Width determines how fast changes with Peclet number as follows:

  - 0.5 at Pe=p.

  - 0.8808 and 0.1192 at Pe=p+w and p-w.

  - 0.9820 and 0.0180 at Pe=p+2w and p-2w.

  - 0.9975 and 0.0025 at Pe=p+3w and p-3w.

  - 0.9997 and 0.0003 at Pe=p+4w and p-4w.

  TANH allows users to effectively remove upwind contribution for lower Pe. In the other extreme, one can enforce user-chosen upwind at all Pe if p < 0.0 and w << 1.0 (ex> p=-1.0, w=1e-10).

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
HybridMethod | {blending | tanh} | BLENDING

###### Hybrid Upwind Shift

Syntax

  Hybrid Upwind Shift {=} Value [ For Equation {conserved_enthalpy | continuity | edc_product | enthalpy | mixture_fraction | nuclei | progress_variable | scalar_variance | second_mixture_fraction | solid_volume_fraction | soot | species | temperature | turbulent_dissipation | turbulent_frequency | turbulent_helmholtz_function | turbulent_kinetic_energy | turbulent_v2 | volume_of_fluid | x_momentum | x_solid_momentum | y_momentum | y_solid_momentum | z_momentum | z_solid_momentum} ]

Summary

  Shifting factor for TANH hybrid approach. Can be specified as a time dependent string function or a constant.

Description

  (see HYBRID UPWIND METHOD description)

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Value | “string” | 0.0

###### Hybrid Upwind Width

Syntax

  Hybrid Upwind Width {=} Value [ For Equation {conserved_enthalpy | continuity | edc_product | enthalpy | mixture_fraction | nuclei | progress_variable | scalar_variance | second_mixture_fraction | solid_volume_fraction | soot | species | temperature | turbulent_dissipation | turbulent_frequency | turbulent_helmholtz_function | turbulent_kinetic_energy | turbulent_v2 | volume_of_fluid | x_momentum | x_solid_momentum | y_momentum | y_solid_momentum | z_momentum | z_solid_momentum} ]

Summary

  Width factor for TANH hybrid approach

Description

  Minimum value for this parameter is 1e-10. (see HYBRID UPWIND METHOD description) Can be specified as a time dependent string function or a constant value.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Value | “string” | 1.0

###### Include Continuity Residual Term

Syntax

  Include Continuity Residual Term [ With Diagnostics ]

Summary

  Include the continuity residual term in transport equations

Description

  Continuity is not exactly satisfied during the momentum solve for variable density flows since the mass flux is lagged while the density is updated with new properties. Including the continuity error in momentum can keep the momentum prediction better behaved. The residual should be on the order of the linear solver tolerance for other equations, but including the term can also make the other solves more robust to a bad continuity solve.

  This term is always included when using VOF or a deforming mesh.

###### Lighthill Tensor Smoothing Iterations

Syntax

  Lighthill Tensor Smoothing Iterations {=} Number

Summary

  Number of smoothing iterations for the divergence of the Lighthill tensor.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Number | integer | –

###### Maximum Number Of Continuity_Momentum Nonlinear Iterations

Syntax

  Maximum Number Of Continuity_Momentum Nonlinear Iterations {=} Number

Summary

  Maximum number of nonlinear iterations to take within the momentum/continuity solve.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Number | integer | 1

###### Maximum Number Of Energy_Species Nonlinear Iterations

Syntax

  Maximum Number Of Energy_Species Nonlinear Iterations {=} Number

Summary

  Maximum number of nonlinear iterations to take within the energy-species grouping.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Number | integer | 1

###### Maximum Number Of Gas_Solid_Momentum Nonlinear Iterations

Syntax

  Maximum Number Of Gas_Solid_Momentum Nonlinear Iterations {=} Number

Summary

  Maximum number of nonlinear iterations to take within the gas/solid momentum sets of equations.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Number | integer | 1

###### Maximum Number Of Kepsilon Nonlinear Iterations

Syntax

  Maximum Number Of Kepsilon Nonlinear Iterations {=} Number

Summary

  Maximum number of nonlinear iterations to take within the k-epsilon turbulence model equations grouping.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Number | integer | 1

###### Maximum Number Of Komega Nonlinear Iterations

Syntax

  Maximum Number Of Komega Nonlinear Iterations {=} Number

Summary

  Maximum number of nonlinear iterations to take within the k-omega turbulence model equations grouping.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Number | integer | 1

###### Maximum Number Of Ksgs Nonlinear Iterations

Syntax

  Maximum Number Of Ksgs Nonlinear Iterations {=} Number

Summary

  Maximum number of nonlinear iterations to take within the ksgs turbulence model equations grouping.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Number | integer | 1

###### Maximum Number Of Mixture Fraction Nonlinear Iterations

Syntax

  Maximum Number Of Mixture Fraction Nonlinear Iterations {=} Number

Summary

  Maximum number of nonlinear iterations to take within the mixture fraction equations grouping.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Number | integer | 1

###### Maximum Number Of Nonlinear Iterations

Syntax

  Maximum Number Of Nonlinear Iterations {=} Number

Summary

  Maximum number of nonlinear iterations to take within the time step of the Fuego region.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Number | integer | 1

###### Maximum Number Of Solid Phase Nonlinear Iterations

Syntax

  Maximum Number Of Solid Phase Nonlinear Iterations {=} Number

Summary

  Maximum number of nonlinear iterations to take within the solid momentum/continuity sets of equations.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Number | integer | 1

###### Maximum Number Of Soot Nuclei Nonlinear Iterations

Syntax

  Maximum Number Of Soot Nuclei Nonlinear Iterations {=} Number

Summary

  Maximum number of nonlinear iterations to take within the soot nuclei equations grouping.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Number | integer | 1

###### Maximum Number Of Species Nonlinear Iterations

Syntax

  Maximum Number Of Species Nonlinear Iterations {=} Number

Summary

  Maximum number of nonlinear iterations for the species equations. If the EDC product transport feature is active, then the SPECIES_PRODUCT nonlinear iteration count should be set instead.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Number | integer | 1

###### Maximum Number Of Species_Product Nonlinear Iterations

Syntax

  Maximum Number Of Species_Product Nonlinear Iterations {=} Number

Summary

  Maximum number of nonlinear iterations to take within the Species/EDC_Product grouping. This is only used if the EDC model is active and the EDC product transport feature is being used.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Number | integer | 1

###### Maximum Number Of V2F Nonlinear Iterations

Syntax

  Maximum Number Of V2F Nonlinear Iterations {=} Number

Summary

  Maximum number of nonlinear iterations to take within the v2f turbulence model equations grouping.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Number | integer | 1

###### Maximum Wall Time

Syntax

  Maximum Wall Time {=} WallTime Hours

Summary

  Specify a maximum wall time to let the simulation end gracefully and output before slurm kills it.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
WallTime | real | Infinite

###### Minimum Number Of Nonlinear Iterations

Syntax

  Minimum Number Of Nonlinear Iterations {=} Number

Summary

  Minimum number of nonlinear iterations to take within the time step of the Fuego region.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Number | integer | 1

###### Nonlinear Residual Norm Tolerance

Syntax

  Nonlinear Residual Norm Tolerance {=} Tolerance [ For Equation {conserved_enthalpy | continuity | edc_product | enthalpy | mixture_fraction | nuclei | progress_variable | scalar_variance | second_mixture_fraction | solid_volume_fraction | soot | species | temperature | turbulent_dissipation | turbulent_frequency | turbulent_helmholtz_function | turbulent_kinetic_energy | turbulent_v2 | volume_of_fluid | x_momentum | x_solid_momentum | y_momentum | y_solid_momentum | z_momentum | z_solid_momentum} ]

Summary

  Nonlinear convergence tolerance within a time step in the Fuego region.

  Values for individual equation sets may be set using the optional token. Using both (in either order):

      NONLINEAR RESIDUAL NORM TOLERANCE = {Real}
      NONLINEAR RESIDUAL NORM TOLERANCE = {Real} FOR EQUATION {Equations}

  Will result in the particular equation set to specified value while all others set to general value.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Tolerance | real | 1.0e-15

###### Nonlinear Stabilization Method

Syntax

  Nonlinear Stabilization Method {=} {commutation_error | none | pointwise_residual_error} [ For Equation {conserved_enthalpy | continuity | edc_product | enthalpy | mixture_fraction | nuclei | progress_variable | scalar_variance | second_mixture_fraction | solid_volume_fraction | soot | species | temperature | turbulent_dissipation | turbulent_frequency | turbulent_helmholtz_function | turbulent_kinetic_energy | turbulent_v2 | volume_of_fluid | x_momentum | x_solid_momentum | y_momentum | y_solid_momentum | z_momentum | z_solid_momentum} ]

Summary

  Specify a artificial viscosity stabilization; default is NONE.

Description

  Values for individual equation sets may be set using optional token. Using both (in either order):

  - NSO METHOD = NSOMethod

  - NSO METHOD = NSOMethod FOR EQUATION Equations

  Will result in the particular equation set to specified value while all others set to general value.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
NSOMethod | {commutation_error | none | pointwise_residual_error} | NO_NSO

###### Omit Density Time Derivative In Continuity Equation

Syntax

  Omit Density Time Derivative In Continuity Equation [ For OmitSteps Steps And Blend In Over BlendSteps Steps ]

Summary

  Remove density time derivative in continuity equation

Description

  Remove the density time derivative from the continuity equation. This feature is required for closed boundary flows with accumulation.

  The optional arguments let you omit it for a certain number of timesteps at the start of the simulation, then gradually include it over a number of steps.

###### Output Nonlinear Residual Field For Equation

Syntax

  Output Nonlinear Residual Field For Equation {conserved_enthalpy | continuity | edc_product | enthalpy | mixture_fraction | nuclei | progress_variable | scalar_variance | second_mixture_fraction | solid_volume_fraction | soot | species | temperature | turbulent_dissipation | turbulent_frequency | turbulent_helmholtz_function | turbulent_kinetic_energy | turbulent_v2 | volume_of_fluid | x_momentum | x_solid_momentum | y_momentum | y_solid_momentum | z_momentum | z_solid_momentum} As ResName [ On Output Block BlockName ]

Summary

  Generates output of nonlinear residuals for the requested equation.

Description

  Provide nonlinear residual for output for specified equation. If the optional output block name is specified, then the residual will only be written to that output block.

Parameter | Value | Default
--- | --- | ---
Equations | {conserved_enthalpy | continuity | edc_product | enthalpy | mixture_fraction | nuclei | progress_variable | scalar_variance | second_mixture_fraction | solid_volume_fraction | soot | species | temperature | turbulent_dissipation | turbulent_frequency | turbulent_helmholtz_function | turbulent_kinetic_energy | turbulent_v2 | volume_of_fluid | x_momentum | x_solid_momentum | y_momentum | y_solid_momentum | z_momentum | z_solid_momentum} | –
ResName | string | –

###### Periodic Constant Momentum Body Source Term

Syntax

  Periodic Constant Momentum Body Source Term {=} ConstSrc1 ConstSrc2 ConstSrc3

Summary

  Add constant body force due to periodic config

Description

  For periodic BCS, commonly a constant body force is applied to drive the flow. This line command allows one to provide a constant body force in three dimensions. If more complex sources are needed, the user sub source term procedure is required.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
ConstSrc | real1 real2 real3 | –

###### Progress Variable Source Evaluation Time

Syntax

  Progress Variable Source Evaluation Time {=} {latest | presolve}

Summary

  Evaluation point for sequences of interdependent progress variable source terms. Either the most recently nonlinear update is used in the order in which the progress variables are solved, or the progress variable source terms are evaluated together presolve.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
EvalTime | {latest | presolve} | –

###### Projection Method

Syntax

  Projection Method {=} {fourth_order | second_order | stabilized | zeroth_order} Smoothing [ With {characteristic | momentum | timestep} Scaling ]

Summary

  Specify choice of projection method.

Description

  The smoothing choice may include zeroth, second, or fourth order. No smoothing (zeroth) may allow pressure-velocity decoupling.

  > The scaling term may be specified. This scaling term is related to the factorization approximation to the inverse of the momentum matrix.

  > Time step scaling may show results that are sensitive to the chosen simulation dt at coarse meshes. This error should vanish as the pressure field approached a linear shape, or refinement is performed. Note that characteristic scaling also has the same error, however, its manifestation is less obvious.

  > The stabilized option uses a fourth order smoothing term and characteristic scaling along with an additional dt stabilizing term.

  > In general, the stabilized and “fourth order smoothing” timestep scaling allows for larger time steps. Characteristic scaling seems to limit CFL to below unity, presumably due to stability loss during nodal projection, i.e., splitting error is .

  > “Momentum Scaling”, uses the diagonal of the momentum equation as the scaling term. While the leading order term with this method will be similar to the timestep scaling scheme, it can sometimes offer better stability since it also includes effects from the other terms in the momentum equation.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
ProjectionMethod | {fourth_order | second_order | stabilized | zeroth_order} | –

###### Randomize Pressure

Syntax

  Randomize Pressure

Summary

  Set a random pressure field for initial guess

Description

  Randomize the initial guess to the linear solve for pressure. The randomization is imposed after the nonlinear residual is computed.

###### Skip Pressure Update If Continuity Solve Fails

Syntax

  Skip Pressure Update If Continuity Solve Fails

Summary

  Do not update the pressure field or mdot if the continuity solve fails

Description

  If the continuity solve fails the resulting pressure delta may be large or non-physical. Activating this option skips the pressure update and mdot update when the solver fails. Repeated solver failures should be watched for in the log file.

  This is a beta feature.

###### Source Term Function

Syntax

  Source Term Function {=} FuncStr For Equation {conserved_enthalpy | continuity | edc_product | enthalpy | mixture_fraction | nuclei | progress_variable | scalar_variance | second_mixture_fraction | solid_volume_fraction | soot | species | temperature | turbulent_dissipation | turbulent_frequency | turbulent_helmholtz_function | turbulent_kinetic_energy | turbulent_v2 | volume_of_fluid | x_momentum | x_solid_momentum | y_momentum | y_solid_momentum | z_momentum | z_solid_momentum} [ VariableName ]

Summary

  Source term string function to use for the given equation. Registered variables with aliases include time (t), spatial coordinates (x,y,z), velocity (u,v,w), density (rho), and pressure (p). Additionally, any valid global variable or nodal variable can be used with its full name. Vector variables, like mass fraction, must be indexed numerically (e.g. “mass_fraction[3]”)

  The function string must be enclosed in quotes if it has spaces or commas. For example: Source Term Function for x_momentum = “min(1, 0.1*t)”

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
FuncStr | “string” | –
Equation | {conserved_enthalpy | continuity | edc_product | enthalpy | mixture_fraction | nuclei | progress_variable | scalar_variance | second_mixture_fraction | solid_volume_fraction | soot | species | temperature | turbulent_dissipation | turbulent_frequency | turbulent_helmholtz_function | turbulent_kinetic_energy | turbulent_v2 | volume_of_fluid | x_momentum | x_solid_momentum | y_momentum | y_solid_momentum | z_momentum | z_solid_momentum} | –

###### Source Term Subroutine

Syntax

  Source Term Subroutine {=} Subroutine For Equation {conserved_enthalpy | continuity | edc_product | enthalpy | mixture_fraction | nuclei | progress_variable | scalar_variance | second_mixture_fraction | solid_volume_fraction | soot | species | temperature | turbulent_dissipation | turbulent_frequency | turbulent_helmholtz_function | turbulent_kinetic_energy | turbulent_v2 | volume_of_fluid | x_momentum | x_solid_momentum | y_momentum | y_solid_momentum | z_momentum | z_solid_momentum} [ VariableName ]

Summary

  Source term user subroutine for the given equation. This is often useful in verification studies where one wishes to use a manufactured solution and must provide source terms for various governing equations.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Subroutine | string | –
Equations | {conserved_enthalpy | continuity | edc_product | enthalpy | mixture_fraction | nuclei | progress_variable | scalar_variance | second_mixture_fraction | solid_volume_fraction | soot | species | temperature | turbulent_dissipation | turbulent_frequency | turbulent_helmholtz_function | turbulent_kinetic_energy | turbulent_v2 | volume_of_fluid | x_momentum | x_solid_momentum | y_momentum | y_solid_momentum | z_momentum | z_solid_momentum} | –

###### Stop Simulation If Peak Velocity Exceeds

Syntax

  Stop Simulation If Peak Velocity Exceeds MaxVel

Summary

  Abort the simulation if velocities get too large.

Description

  By default Fuego will continue time stepping as the simulation diverges and will go until velocities overflow or solvers start returning NaN or Inf.

  If you want it to stop sooner than that, you can set a peak velocity magnitude to abort at.

Parameter | Value | Default
--- | --- | ---
MaxVel | real | infinity

###### Under Relax

Syntax

  Under Relax {conserved_enthalpy | continuity | edc_product | enthalpy | mixture_fraction | nuclei | progress_variable | scalar_variance | second_mixture_fraction | solid_volume_fraction | soot | species | temperature | turbulent_dissipation | turbulent_frequency | turbulent_helmholtz_function | turbulent_kinetic_energy | turbulent_v2 | volume_of_fluid | x_momentum | x_solid_momentum | y_momentum | y_solid_momentum | z_momentum | z_solid_momentum} By Urf [ With Implicit Term ]

Summary

  Under relaxation factor for the given equation.

Description

  Implicit relaxation is applied to the momentum equations. Explicit relaxation is applied to the pressure update. Transport equations are relaxed explicitly unless the “WITH IMPLICI TERM” option is used.

  Under-relaxation can be a constant value or a function of time (t). If the function used has spaces or commas, it should be enclosed in quotes. The value will be internally clipped between 1e-6 and 1.

Parameter | Value | Default
--- | --- | ---
Equations | {conserved_enthalpy | continuity | edc_product | enthalpy | mixture_fraction | nuclei | progress_variable | scalar_variance | second_mixture_fraction | solid_volume_fraction | soot | species | temperature | turbulent_dissipation | turbulent_frequency | turbulent_helmholtz_function | turbulent_kinetic_energy | turbulent_v2 | volume_of_fluid | x_momentum | x_solid_momentum | y_momentum | y_solid_momentum | z_momentum | z_solid_momentum} | –
Urf | “string” | 1.0

###### Under Relax Momentum By

Syntax

  Under Relax Momentum By Urf

Summary

  Under relaxation factor for the momentum equations.

  Under-relaxation can be a constant value or a function of time (t). If the function used has spaces or commas, it should be enclosed in quotes. The value will be internally clipped between 1e-6 and 1.

Parameter | Value | Default
--- | --- | ---
Urf | “string” | –

###### Under Relax Pressure By

Syntax

  Under Relax Pressure By Urf

Summary

  Under relaxation factor for the pressure. This is equivalent to specifying an URF on continuity, and is provided for backward compatibility.

  Under-relaxation can be a constant value or a function of time (t). If the function used has spaces or commas, it should be enclosed in quotes. The value will be internally clipped between 1e-6 and 1.

Parameter | Value | Default
--- | --- | ---
Urf | “string” | –

###### Under Relax Solid_Momentum By

Syntax

  Under Relax Solid_Momentum By Urf

Summary

  Under relaxation factor for the solid-phase momentum equations.

  Under-relaxation can be a constant value or a function of time (t). If the function used has spaces or commas, it should be enclosed in quotes. The value will be internally clipped between 1e-6 and 1.

Parameter | Value | Default
--- | --- | ---
Urf | “string” | –

###### Under Relax Temperature_Extraction By

Syntax

  Under Relax Temperature_Extraction By Urf

Summary

  Under relaxation factor for the temperature extraction from enthalpy

Description

  Relax the temperature computed from the enthalpy. This gives a temperature that is not entirely consistent with the current state (composition and enthalpy), and will destroy time-accuracy unless sufficient Picard loops are taken. However, it may be useful for steady-state computations where species and energy equations are not being coupled strongly or solved accurately.

  > Under-relaxation can be a constant value or a function of time (t). If the function used has spaces or commas, it should be enclosed in quotes. The value will be internally clipped between 1e-6 and 1.

Parameter | Value | Default
--- | --- | ---
Urf | “string” | –

###### Upwind Limiter

Syntax

  Upwind Limiter {=} {minmod | none | superbee | van_albada | van_leer} [ For Equation {conserved_enthalpy | continuity | edc_product | enthalpy | mixture_fraction | nuclei | progress_variable | scalar_variance | second_mixture_fraction | solid_volume_fraction | soot | species | temperature | turbulent_dissipation | turbulent_frequency | turbulent_helmholtz_function | turbulent_kinetic_energy | turbulent_v2 | volume_of_fluid | x_momentum | x_solid_momentum | y_momentum | y_solid_momentum | z_momentum | z_solid_momentum} ]

Summary

  Specify a limiter for convection operator; default is SUPERBEE.

Description

  Limiter functions are valid only for the MUSCL scheme.

  Values for individual equation sets may be set using optional token. Using both (in either order):

  - UPWIND LIMITER = UpwindLimiter

  - UPWIND LIMITER = UpwindLimiter FOR EQUATION Equations

  Will result in the particular equation set to specified value while all others set to general value.

  Note: Rotational invariance of the code is not expected while using a limiter function.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
UpwindLimiter | {minmod | none | superbee | van_albada | van_leer} | SUPERBEE

###### Upwind Method

Syntax

  Upwind Method {=} {lps | muscl | upw} [ For Equation {conserved_enthalpy | continuity | edc_product | enthalpy | mixture_fraction | nuclei | progress_variable | scalar_variance | second_mixture_fraction | solid_volume_fraction | soot | species | temperature | turbulent_dissipation | turbulent_frequency | turbulent_helmholtz_function | turbulent_kinetic_energy | turbulent_v2 | volume_of_fluid | x_momentum | x_solid_momentum | y_momentum | y_solid_momentum | z_momentum | z_solid_momentum} ]

Summary

  Upwind method for convective terms

Description

  All methods are hybrid in the sense that a centered scheme is blended based on the local Peclet number.

  Values for individual equation sets may be set using optional token. Using both (in either order):

  - UPWIND METHOD = UpwindMethod

  - UPWIND METHOD = UpwindMethod FOR EQUATION Equations

  Will result in the particular equation set to specified value while all others set to general value.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
UpwindMethod | {lps | muscl | upw} | LPS

###### Use Equation Solver

Syntax

  Use Equation Solver SolverName For Equation {conserved_enthalpy | continuity | edc_product | enthalpy | mixture_fraction | nuclei | progress_variable | scalar_variance | second_mixture_fraction | solid_volume_fraction | soot | species | temperature | turbulent_dissipation | turbulent_frequency | turbulent_helmholtz_function | turbulent_kinetic_energy | turbulent_v2 | volume_of_fluid | x_momentum | x_solid_momentum | y_momentum | y_solid_momentum | z_momentum | z_solid_momentum}

Summary

  Link an equation solver to an equation set.

Description

  For example, if a solver block “scalar” was created using the Tpetra package, e.g., BEGIN TPETRA EQUATION SOLVER scalar and the equation set was the u-component of momentum then the line command would be as follows: USE EQUATION SOLVER scalar FOR EQUATION X-Momentum.

  This command can be omitted, and a default solver will be assigned (either the HIGH_ASPECT_CONTINUITY or SCALAR_TRANSPORT preset solvers). The default continuity solver is GMRES with the MueLu preconditioner and the default scalar transport solver is GMRES with the SGS preconditioner.

Parameter | Value | Default
--- | --- | ---
SolverName | string | –
Equations | {conserved_enthalpy | continuity | edc_product | enthalpy | mixture_fraction | nuclei | progress_variable | scalar_variance | second_mixture_fraction | solid_volume_fraction | soot | species | temperature | turbulent_dissipation | turbulent_frequency | turbulent_helmholtz_function | turbulent_kinetic_energy | turbulent_v2 | volume_of_fluid | x_momentum | x_solid_momentum | y_momentum | y_solid_momentum | z_momentum | z_solid_momentum} | –

###### Use External Continuity Source

Syntax

  Use External Continuity Source

Summary

  Add external species source term from a transfer

Description

  Add source terms to the continuity equation from a nodal field transferred to this region, e.g. from a Fuego particle region. The field continuity_source will be added to the RHS of the continuity equation; this fields should have units of rate-of-change of mass per volume, so that multiplication by the control volume gives the correct source term. The transfer operation should send to the variables at state “none”.

###### Use External Energy Source

Syntax

  Use External Energy Source

Summary

  Add external energy source term from a transfer

Description

  Add source terms to the temperature or enthalpy equations from a nodal field transferred to this region, e.g. from a Fuego particle region. The field energy_source will be added to the RHS of the energy equation; this fields should have units of rate-of-change of energy per volume, so that multiplication by the control volume gives the correct source term. The transfer operation should send to the variables at state “none”.

###### Use External Mixture_Fraction Source

Syntax

  Use External Mixture_Fraction Source

Summary

  Add external species source term from a transfer

Description

  Add source terms to the mixture fraction equation from a nodal field transferred to this region, e.g. from a Fuego particle region. The field mixture_fraction_source will be added to the RHS of the mixture fraction equation; this fields should have units of rate-of-change of mass per volume, so that multiplication by the control volume gives the correct source term. The transfer operation should send to the variables at state “none”.

###### Use External Momentum Source

Syntax

  Use External Momentum Source

Summary

  Add external momentum source terms from a transfer

Description

  Add source terms to the momentum equations from a nodal field transferred to this region, e.g. from a Fuego particle region. The fields x_momentum_source, y_momentum_source, and z_momentum source will be added to the RHS of the momentum equations; these fields should have units of rate-of-change of momentum per volume, so that multiplication by the control volume gives the correct source term. The transfer operation should send to the variables at state “none”.

###### Use External Soot_Mass_Fraction Source

Syntax

  Use External Soot_Mass_Fraction Source

Summary

  Add external soot source term from a transfer

Description

  Add source terms to the soot mass fraction equation from a nodal field transferred to this region, e.g. from a Fuego particle region. The field soot_mass_fraction_source will be added to the RHS of the soot mass fraction equation; this fields should have units of rate-of-change of mass per volume, so that multiplication by the control volume gives the correct source term. The transfer operation should send to the variables at state “none”.

###### Use External Species Source

Syntax

  Use External Species Source

Summary

  Add external species source term from a transfer

Description

  Add source terms to the species equations from a nodal field transferred to this region, e.g. from a Fuego particle region. The vector field species_source will be added to the RHS of the species equation; this fields should have units of rate-of-change of mass of species i per volume, so that multiplication by the control volume gives the correct source term. The transfer operation should send to the variables at state “none”.

###### Use Lumped Velocity Density Interpolation

Syntax

  Use Lumped Velocity Density Interpolation

Summary

  Interpolate the density-velocity product

Description

  By default the continuity equation interpolates velocity and density separately to sub-control surfaces. This option interpolates the product of density times velocity instead.

###### Use Radiation Source From External Region

Syntax

  Use Radiation Source From External Region [ Using Classic Linearization ]

Summary

  Add in a source term from participating-media radiation which comes from another region through a transfer.

  The USING CLASSIC LINEARIZATION optional argument is no longer used or needed, and will be removed in a future release.

###### Use Shifted Density Iteration

Syntax

  Use Shifted Density Iteration

Summary

  Use a lagged density in the momentum solve but an updated density in the velocity projection

Description

  Use a lagged density for momentum solve relative to the velocity projection similar to https://doi.org/10.1016/j.jcp.2012.01.027

  This is a beta feature.

###### Use Skew Symmetric Central Operator

Syntax

  Use Skew Symmetric Central Operator [ For Equation {conserved_enthalpy | continuity | edc_product | enthalpy | mixture_fraction | nuclei | progress_variable | scalar_variance | second_mixture_fraction | solid_volume_fraction | soot | species | temperature | turbulent_dissipation | turbulent_frequency | turbulent_helmholtz_function | turbulent_kinetic_energy | turbulent_v2 | volume_of_fluid | x_momentum | x_solid_momentum | y_momentum | y_solid_momentum | z_momentum | z_solid_momentum} ]

Summary

  The blended central operator will be skew symmetric, default is .

Description

  The convection operator is always blended with pure central (see hybrid factor description). For the CVFEM methodology, there is a balance between stability and accuracy. Dotting the momentum equation with velocity and summing yields the kinetic energy equation. If the convection operator is skew symmetric, than this dot product leaves something that is perfectly zero. This means that there can be no generation of kinetic energy and simulations can remain stable.

  The full CVFEM stencil (27-pt on a hex mesh) is not skew symmetric. Therefore, in cases where one uses pure central (by specifying a hybrid factor of unity) there can be issues - especially on coarse meshes.

## 7.7.10. Buoyancy Model Specification

Scope

  Solution Options

Summary

  Specify buoyancy modeling options.

    begin Buoyancy Model Specification BuoyModelName

       Buoyancy Model {=} {boussinesq | buoyant | concentration | differential | no_buoyancy}

       Buoyancy Reference VarName {=} Value

       Buoyancy Reference Mass_Fraction Species {=} y0

       Buoyancy Reference Mole_Fraction Species {=} x0

       Buoyancy Source Term {=} {consistent | default | lumped}

    end Buoyancy Model Specification BuoyModelName

### 7.7.10.1. Line Commands

###### Buoyancy Model

Syntax

  Buoyancy Model {=} {boussinesq | buoyant | concentration | differential | no_buoyancy}

Summary

  Specification of Buoyancy model to be used in momentum equations.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
BuoyancyModel | {boussinesq | buoyant | concentration | differential | no_buoyancy} | NO_BUOYANCY

###### Buoyancy Reference

Syntax

  Buoyancy Reference VarName {=} Value

Summary

  Buoyancy reference value for the given field.

Description

  If the selected buoyancy model requires material property calculations, then reference values must be specified for all input variables required by the particular material model. In the typical case where Cantera is used for property evaluation, then reference properties must be specified for “temperature”, “pressure”, and “mass_fraction”. Other material models may have different dependencies.

Parameter | Value | Default
--- | --- | ---
VarName | string | –
{=} | {= | are | is} | –
Value | real | –

###### Buoyancy Reference Mass_Fraction

Syntax

  Buoyancy Reference Mass_Fraction Species {=} y0

Summary

  Buoyancy reference mass fraction for calculating density.

Description

  If the selected buoyancy model requires material property calculations, then reference values must be specified for all input variables required by the particular material model. In the typical case where Cantera is used for property evaluation, then reference properties must be specified for “temperature”, “pressure”, and “mass_fraction”. Other material models may have different dependencies.

Parameter | Value | Default
--- | --- | ---
Species | string | –
{=} | {= | are | is} | –
y0 | real | –

###### Buoyancy Reference Mole_Fraction

Syntax

  Buoyancy Reference Mole_Fraction Species {=} x0

Summary

  Buoyancy reference mole fraction for calculating density.

Description

  If the selected buoyancy model requires material property calculations, then reference values must be specified for all input variables required by the particular material model. In the typical case where Cantera is used for property evaluation, then reference properties must be specified for “temperature”, “pressure”, and “mass_fraction”. Other material models may have different dependencies.

Parameter | Value | Default
--- | --- | ---
Species | string | –
{=} | {= | are | is} | –
x0 | real | –

###### Buoyancy Source Term

Syntax

  Buoyancy Source Term {=} {consistent | default | lumped}

Summary

  Specifies if the buoyancy source term should be lumped, consistent, or the same as the mass matrix.

Description

  Using a lumped source term diagonalizes the mass matrix contribution to the linear system, and therefore results in a more diagonally-dominant matrix. This under-integration of the source term may result in more monotonic behavior for certain problems.

  Using a different source term and mass matrix lumping may introduce undesirable behavior near high gradient regions. Default behavior is to use the same approach for the mass matrix and buoyancy source term.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
BuoyancySourceTermType | {consistent | default | lumped} | DEFAULT

## 7.7.11. Edc Model Specification

Scope

  Solution Options

Summary

  Specify EDC combustion model options.

    begin Edc Model Specification EdcSpecName

       Activate Absorption Model

       Activate Co2 Dissociation Model

       Activate Hydrogen Dissociation Model

       Activate Separate Co Irreversible Oxidation Pathway

       Characteristic Length Scale For Absorption Coefficient Determination {=} CharacteristicLength

       Critical Damkohler Number For Suppression {=} dacrit

       Edc Fuel Name {=} Fuel

       Edc Ignition Threshold Temperature {=} IgnTemp

       Edc Ignition Time {=} Igntime

       Edc Minimum Product Fraction {=} Prmin

       Edc Reaction Time Scale {=} Tchem

       Include Edc Laminar Limit Model

       Minimum Soot Production Temperature {=} Tsootmin

       Omit Near Wall Combustion

       Use Edc Product Transport

       Use Explicit Treatment Of Edc Source Terms

       Use Pure Oxygen For Oxidizer Mixture

       Use Sintef Soot Model

    end Edc Model Specification EdcSpecName

### 7.7.11.1. Line Commands

###### Activate Absorption Model

Syntax

  Activate Absorption Model

Summary

  Calculate absorption coefficient for use in conjunction with radiation calculations. This will also ensure that the rte source term includes the convolution over gamma chi. If a rte block is active, you may also elect to compute the rte source term by the use of mean temperatures.

###### Activate Co2 Dissociation Model

Syntax

  Activate Co2 Dissociation Model

Summary

  Include effects of CO2 dissociation into CO and O2 at high temperatures

Description

  At high temperatures, the equilibrium between CO2, CO, and O2 shifts away from CO2, which can significantly decrease the flame temperature. Activating this model will add this effect to the standard EDC combustion model.

###### Activate Hydrogen Dissociation Model

Syntax

  Activate Hydrogen Dissociation Model

Summary

  Include effects of H2 dissociation into H

Description

  At temperatures greater than about 2000K, the equilibrium between H2 and H will yield non-negligible concentrations of H which can significantly decrease flame temperatures. Activating this model will add this effect to the standard EDC combustion model using the correlations of W.W. Erikson, which are derived from the NASA CEA code [242, 243].

  Note that the H species must be included in the Cantera input XML file, and neither H nor H2 should be the “last” species in the list since this species is not independent of the rest (to enforce unity sum) and may be susceptible to more noise than the others. Since temperature and other properties are very sensitive to oscillations in the H and H2 equilibrium, this noise could be problematic.

###### Activate Separate Co Irreversible Oxidation Pathway

Syntax

  Activate Separate Co Irreversible Oxidation Pathway

Summary

  Add CO oxidation pathway as a separate reaction pathway. This should really be used only in the context of a propellant fire in the presence of hydrogen combustion.

###### Characteristic Length Scale For Absorption Coefficient Determination

Syntax

  Characteristic Length Scale For Absorption Coefficient Determination {=} CharacteristicLength

Summary

  Override the absorption coefficient normally calculated by fuego with this value.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
CharacteristicLength | real | –

###### Critical Damkohler Number For Suppression

Syntax

  Critical Damkohler Number For Suppression {=} dacrit

Summary

  Critical Damkohler number at which suppression is activated. A value of 0.0 denotes no suppression.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
dacrit | real | 0.0

###### Edc Fuel Name

Syntax

  Edc Fuel Name {=} Fuel

Summary

  The name of the EDC fuel species, typically either H2 or a major hydrocarbon

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Fuel | string | –

###### Edc Ignition Threshold Temperature

Syntax

  Edc Ignition Threshold Temperature {=} IgnTemp

Summary

  The temperature below which the ignition model is activated

Description

  If the ignition model is requested (through the IGNITE initial condition keyword), then it will be activated if all temperatures in the corresponding initial condition block are below this temperature.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
IgnTemp | real | 1000.0 K

###### Edc Ignition Time

Syntax

  Edc Ignition Time {=} Igntime

Summary

  The time at which the EDC combustion model is activated. No combustion will occur before this time.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Igntime | real | 0.0

###### Edc Minimum Product Fraction

Syntax

  Edc Minimum Product Fraction {=} Prmin

Summary

  The minimum product fraction, below which the EDC model will be deactivated.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Prmin | real | 1.0e-6

###### Edc Reaction Time Scale

Syntax

  Edc Reaction Time Scale {=} Tchem

Summary

  Reaction time scale to set extinction

Description

  Characteristic time scale of the chemical kinetics. Residence time in the fine structure region will be compared to this to determine if extinction will result.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Tchem | real | 7.0e-5

###### Include Edc Laminar Limit Model

Syntax

  Include Edc Laminar Limit Model

Summary

  Turn on the EDC laminar limit model for low-turbulence situations

Description

  Turn on the EDC laminar limit model. This model requires setting three model constants: CtauLam, CgammaLam, and ClamTrans. The model uses a time scale based on a velocity gradient rather than the turb_ke/turb_diss. This appropriate time scale permits the flame to anchor in laminar regions.

###### Minimum Soot Production Temperature

Syntax

  Minimum Soot Production Temperature {=} Tsootmin

Summary

  The minimum temperature for which we allow soot to be produced.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Tsootmin | real | 300.0 K

###### Omit Near Wall Combustion

Syntax

  Omit Near Wall Combustion

Summary

  Disables combustion near the wall nodes by setting the production rate to zero. This prevents the values calculated for the EDC combustion rate to be added to the wall element.

###### Use Edc Product Transport

Syntax

  Use Edc Product Transport

Summary

  Solve a transport equation for the EDC reaction products.

Description

  If any of the “product” species (CO2 or H2O for a hydrocarbon fuel, or H2O for hydrogen fuel) are to be injected into the domain either through a boundary condition or initial condition to simulate a diluent stream or ambient concentration, then the EDC model will be unable to differentiate which portion of the product species originated directly from combustion and which did not. This can badly distort the EDC model reaction rate calculation and yield incorrect results.

  This option solves a transport equation for EDC products that were generated through combustion rather than evaluating it directly from local mass fractions, eliminating issues with product species injection. (If no product species are being injected, then identical results can be obtained at a lower cost without this option.)

  To use this feature, activate this line command and also activate the EDC_Product equation along with the Species equation. Note that no initial or boundary conditions are needed for the EDC_Product equation since it has its own internally-handled special needs. (Any specified initial or boundary conditions will be ignored.)

  Also note that a pilot stream will be unable to ignite a flame when using this model. It will be treated as an inert diluent stream, so that the normal ignition model will be required to ignite the flame. This model in its current form should not be used for piloted flames.

###### Use Explicit Treatment Of Edc Source Terms

Syntax

  Use Explicit Treatment Of Edc Source Terms

Summary

  Allow no implicit treatment of EDC combustion source terms

Description
  The general form of the EDC combustion model for species is

    where rate is a function of gammachi and residence times. This option specifies that the full source term be placed on the right hand side of the species transport equation, e.g., math:rhs+= rate*(Y_{fs,k} - Y_k) as opposed to: and . The user will recall that the transport equations are solved in residual form, hence the above rhs form.

###### Use Pure Oxygen For Oxidizer Mixture

Syntax

  Use Pure Oxygen For Oxidizer Mixture

Summary

  Use pure oxygen as the oxidizer mixture rather than air

Description

  By default, the EDC model assumes a 3.76 N2:O2 ratio for the oxidizer mixture. This option switches to pure O2 as the oxidizer.

###### Use Sintef Soot Model

Syntax

  Use Sintef Soot Model

Summary

  Use the SINTEF soot model instead of the standard soot model.

## 7.7.12. Multiphase Model Specification

Scope

  Solution Options

Summary

  Specify a number of physical parameters that are to be used for multi-phase flow simulations.

    begin Multiphase Model Specification DefinitionName

       Compute Gas Phase Volume Fraction Using GasVolFracEnum1[ GasVolFracEnum2]

       Enable Porous Media Model

       Multiphase {compaction_modulus | density | effective_viscosity_multiplier | maximum_packing_diameter | particle_diameter | reference_elastic_modulus | solid_velocity | soot_density | turbulent_schmidt_number} {=} Values

    end Multiphase Model Specification DefinitionName

### 7.7.12.1. Line Commands

###### Compute Gas Phase Volume Fraction Using

Syntax

  Compute Gas Phase Volume Fraction Using GasVolFracEnum1[ GasVolFracEnum2]

Summary

  Compute the gas phase volume fraction based on soot and particle volume fraction.

Parameter | Value | Default
--- | --- | ---
GasVolFracEnum | {particle | soot} | –

###### Enable Porous Media Model

Syntax

  Enable Porous Media Model

Summary

  Invoke porous media (aka clutter model, Darcy flow) model equations; an initial condition for gas volume fraction is expected, however, defaulted to unity.

###### Multiphase

Syntax

  Multiphase {compaction_modulus | density | effective_viscosity_multiplier | maximum_packing_diameter | particle_diameter | reference_elastic_modulus | solid_velocity | soot_density | turbulent_schmidt_number} {=} Values

Summary

  Specify parameters for multi-phase simulations.

Description

  These values are used in solid and gas phase transport equations

Parameter | Value | Default
--- | --- | ---
MultiPhaseParams | {compaction_modulus | density | effective_viscosity_multiplier | maximum_packing_diameter | particle_diameter | reference_elastic_modulus | solid_velocity | soot_density | turbulent_schmidt_number} | –
{=} | {= | are | is} | –
Values | real | –

## 7.7.13. Radiation Transport Equation Model Specification

Scope

  Solution Options

Summary

  Specify options for radiation model.

    begin Radiation Transport Equation Model Specification RadModelName

       Absorption Coefficient Model {=} {leckner}

       Aluminum_Oxide Emittance Model {=} {brewster | konopka | table}

       Characteristic Length Scale For Absorption Coefficient Determination {=} CharacteristicLength

       Species Name For {aluminum_oxide | carbon_dioxide | hydrogen_chloride | soot | water} {=} SpeciesName

       Subgrid Mixing Model {=} {no_subgrid_mixing}

    end Radiation Transport Equation Model Specification RadModelName

### 7.7.13.1. Line Commands

###### Absorption Coefficient Model

Syntax

  Absorption Coefficient Model {=} {leckner}

Summary

  Specify absorption coefficient model

Description

  This option will allow for the specification of an absorption coefficient model. At present, only the Leckner model is supported and is, therefore, the default. Specification of the model requires designation of water and carbon dioxide string names.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
AbsorpCoeffModel | {leckner} | LECKNER

###### Aluminum_Oxide Emittance Model

Syntax

  Aluminum_Oxide Emittance Model {=} {brewster | konopka | table}

Summary

  Specify alumina emittance model

Description

  This option allows for the specification of an absorption coefficient model for alumina. Konopka and Table (user-specified) are also available. For the table model, the user must have T-ABS-MODEL.txt file in the current directory with the following format:

  0.000094

  4

  300.0 0.0821

  1000.0 0.1064

  2320.0 0.0024

  10000.0 0.7435

  Where:

  0.000094 is DTHTWO (Characteristic diameter of Al2O3 Units: [cm]). 4 is the number of points in the linear interpolation absorption model (Absorption as function of temperature). The remaining lines are T, ABS points for the model. Linear interpolation is used between the points. For T less than T_0 (lowest temperature for these points), ABS = ABS(T_0). For T greater than T_0 (highest temperature for these points), ABS = ABS(T_0).

  Brewster and Konopka options are equivalent to Table option with:

  Konopka:

  0.000094

  4

  300 0.0821

  1000 0.10639

  2320 0.002384

  2320.001 0.04 (at , this represents a discontinuous change in absorption coefficient)

  Brewster:

  0.000094

  4

  300 0.0821

  1000 0.10639

  2320 0.002384

  10000 0.74352 ( is set high enough that particle temperature is not likely to be this high)

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
AluminaEmittModel | {brewster | konopka | table} | brewster

###### Characteristic Length Scale For Absorption Coefficient Determination

Syntax

  Characteristic Length Scale For Absorption Coefficient Determination {=} CharacteristicLength

Summary

  Override the absorption coefficient normally calculated by fuego with this value.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
CharacteristicLength | real | –

###### Species Name For

Syntax

  Species Name For {aluminum_oxide | carbon_dioxide | hydrogen_chloride | soot | water} {=} SpeciesName

Summary

  Specify string names that map to water, carbon dioxide, hydrogen chloride or aluminum oxide (AKA alumina)

Description

  This option will allow for the specification of an absorption coefficient model specification. At present, only the Leckner model is supported for water and carbon dioxide. Hydrogen chloride and aluminum oxide (alumina) provided by tables.

Parameter | Value | Default
--- | --- | ---
AbsorpCoeffSpecies | {aluminum_oxide | carbon_dioxide | hydrogen_chloride | soot | water} | –
{=} | {= | are | is} | –
SpeciesName | string | –

###### Subgrid Mixing Model

Syntax

  Subgrid Mixing Model {=} {no_subgrid_mixing}

Summary

  Specify subgrid mixing model for RTE source term

Description

  This option will allow for the specification of subgrid mixing model. At present, there is no model supported other than to ignore fluctuation effects, which is the default.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
RTESubgridModel | {no_subgrid_mixing} | no_subgrid_mixing

## 7.7.14. Time Integration Specification

Scope

  Solution Options

Summary

  Specify time integration options. Either BDF2 or BDF1.

    begin Time Integration Specification TimeIntSpecName

       Activate Bdf2 [ After Step BDF2StartStep  ]

       Mass Matrix {=} {consistent | lumped}

       Predictor Algorithm {=} {adams_bashforth | forward_euler | simple}

       Use Second Order Implicit Time Integration [ With Blending Coefficient {=} BlendCoeff  ]

    end Time Integration Specification TimeIntSpecName

### 7.7.14.1. Line Commands

###### Activate Bdf2

Syntax

  Activate Bdf2 [ After Step BDF2StartStep ]

Summary

  Activation of the second-order BDF2 time integrator.

Description

  BDF2 is a A-stable, three state time integrator that has been demonstrated to be well performing in the low-Mach application space. When activated, all PDEs with time terms will use BDF2. The user specification for MASS MATRIX is used to determine the usage of the lumped or consistent form.

  Use the optional argument to delay the use of BDF2 for some number of time steps. Backward euler will be used for those time steps instead.

###### Mass Matrix

Syntax

  Mass Matrix {=} {consistent | lumped}

Summary

  Specifies if the mass matrix (also known as the capacitance matrix) is to be lumped using row sum rule.

Description

  Using a lumped mass matrix diagonalizes the mass matrix contribution to the linear system, and therefore results in a more diagonally-dominant matrix. This under-integration of the mass matrix may result in more monotonic behavior for certain problems.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
MassMatrixType | {consistent | lumped} | LUMPED

###### Predictor Algorithm

Syntax

  Predictor Algorithm {=} {adams_bashforth | forward_euler | simple}

Summary

  Specification of predictor algorithm

Description

  Three predictor algorithms are supported, i.e.,

  - Simple Predictor:

  - Forward Euler:

  - Adams Bashforth: .

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
PredictorAlgorithm | {adams_bashforth | forward_euler | simple} | –

###### Use Second Order Implicit Time Integration

Syntax

  Use Second Order Implicit Time Integration [ With Blending Coefficient {=} BlendCoeff ]

Summary

  Deprecated.

Description

  Crank-Nicholson scheme is deprecated, defaults to BDF2.

## 7.7.15. Turbulence Model Specification

Scope

  Solution Options

Summary

  Specify turbulence modeling options.

    begin Turbulence Model Specification TurbSpecName

       Activate Deris Flaming Buoyancy Source Term

       Activate Deris Nonflaming Buoyancy Source Term

       Activate Rodi Buoyancy Source Term

       Activate Rodi Density Buoyancy Source Term

       Determine Utau Via Nonlinear Law Of The Wall Iteration

       Force Constant Scalar Variance Coefficient

       Include Molecular Viscosity In K-E Diffusion Coefficient

       Limit Turbulent Ke Production To Value Times Dissipation

       Omit Low Reynolds Turbulence Dissipation Source Term

       Omit Near Wall Turbulent Ke Transport Equation

       Omit Turbulence Source Terms On Block(S) BlockList...

       Omit Velocity Divergence In Turbulent Production Term

       Time Filter {=} Value

       Turbulence Model {=} {dksgs | dsmag | inagaki_ksgs | ke | ksgs | kw | lam | lrke | lrkw | lrsst | rng | smag | sst | sstdes | v2f}

       Turbulence Model Parameter {frequency_scaling | kappa | minimum_k | yplus_crit} {=} Value

       Turbulence Postprocessor {=} {q_criterion | residual_reynolds_stress | resolved_reynolds_stress}

       Under Relax Turbulent_Viscosity By Urf

       Use Buoyant Vorticity Generation At Value Seconds

       Use Dynamic Ksgs

       Wall Distance Band Size {=} BandSize

       Wall Model {=} {modeled | resolved}

    end Turbulence Model Specification TurbSpecName

### 7.7.15.1. Line Commands

###### Activate Deris Flaming Buoyancy Source Term

Syntax

  Activate Deris Flaming Buoyancy Source Term

Summary

  Add de Ris’ flaming buoyancy source term to turbulence transport equations.

Description

  This option adds the buoyancy source term of Rodi to the turbulent kinetic energy equation (for all turbulence models) and to some extent, to the dissipation rate equation. Two versions - flaming and non-flaming - are proposed in the paper. The source term of the flaming version is given by where is a user-defined coefficient. The coefficient is set 0.01 for now without sufficient validation efforts.

  Reference: JL de Ris, Procedia Engineering 62(2013)13-27

###### Activate Deris Nonflaming Buoyancy Source Term

Syntax

  Activate Deris Nonflaming Buoyancy Source Term

Summary

  Add de Ris’ non-flaming buoyancy source term to turbulence transport equations.

Description

  This option adds the buoyancy source term of Rodi to the turbulent kinetic energy equation (for all turbulence models) and to some extent, to the dissipation rate equation. Non-flaming version is a combination of BVG (Buoyant Vorticity Generation) and Rodi models. The source term is given by where is a user-defined coefficient. The coefficient is set 0.01 for now without sufficient validation efforts.

  Reference: JL de Ris, Procedia Engineering 62(2013)13-27

###### Activate Rodi Buoyancy Source Term

Syntax

  Activate Rodi Buoyancy Source Term

Summary

  Add Rodi’s buoyancy source term to turbulence transport equations.

Description

  This option adds the buoyancy source term of Rodi to the turbulent kinetic energy equation (for all turbulence models) and in some cases, the dissipation rate equation. The source term is given by, For the turbulent kinetic energy, augments the right hand side while for the dissipation rate equation, is the augmented right hand side term. The source term is limited to a fraction of the dissipation rate.

  This model has not been validated for use in the context of turbulence models other than the standard - model.

###### Activate Rodi Density Buoyancy Source Term

Syntax

  Activate Rodi Density Buoyancy Source Term

Summary

  Add Rodi’s buoyancy source term to turbulence transport equations, modified to be density based

Description

  This option adds the buoyancy source term of Rodi to the turbulent kinetic energy equation (for all turbulence models) and in some cases, the dissipation rate equation. The source term is given by, For the turbulent kinetic energy, augments the right hand side while for the dissipation rate equation, is the augmented right hand side term. The source term is limited to a fraction of the dissipation rate.

  This model is equivalent to the standard rodi model for single component, thermal plumes.

###### Determine Utau Via Nonlinear Law Of The Wall Iteration

Syntax

  Determine Utau Via Nonlinear Law Of The Wall Iteration

Summary

  Use law of the wall nonlinear iteration for utau calculation

Description

  Elect to perform a nonlinear iteration of the law-of-the-wall formula to calculate utau, the wall friction velocity at the boundary integration points. This value will be used to calculate the modeled wall shear stress and, when activated, the modeled wall heat flux. Alternatively, the friction velocity will be calculated from the nodal value of turbulent k.e. that may be approximated when a turbulent kinetic energy transport equation is not solved.

###### Force Constant Scalar Variance Coefficient

Syntax

  Force Constant Scalar Variance Coefficient

Summary

  Keep the algebraic scalar variance coefficient constant while using a dynamic model

Description

  This option forces a constant coefficient for “Cv” of the algebraic scalar variance model, specified in the global constants block, regardless of use of a dynamic model.

###### Include Molecular Viscosity In K-E Diffusion Coefficient

Syntax

  Include Molecular Viscosity In K-E Diffusion Coefficient

Summary

  Augment diffusion coefficient in turbulence equations via molecular viscosity

Description

  The standard k-e model does not include the molecular viscosity in the diffusion term. This option adds the molecular viscosity to . The line command is also appropriate for the Ksgs and v2-f model.

###### Limit Turbulent Ke Production

Syntax

  Limit Turbulent Ke Production To Value Times Dissipation

Summary

  Choose to limit production source terms

Description

  This option limits the turbulent ke production to a scale factor of dissipation, prod = min(prod, limit*den*en1). In practice, the ratio of production to dissipation is not very high. In some flows, it is useful to specify a value of approximately 1000. The ratio should be checked as part of the analysis to make sure that violation of the physical ratio has not been done. In general, this option is only activated in domain locations where dissipation rate is very small. (Default: 1.0e8)

Parameter | Value | Default
--- | --- | ---
Value | real | –

###### Omit Low Reynolds Turbulence Dissipation Source Term

Syntax

  Omit Low Reynolds Turbulence Dissipation Source Term

Summary

  Remove low Reynolds source term from dissipation rate equation.

Description

  This option removes the low Reynolds number source term from the dissipation rate equation given by Launder and Sharma. The form is .

  This source term is calculated using a two pass shape function evaluation. The first pass calculates the standard derivatives, . The second pass assumes a piecewise constant interpolation of the standard derivatives from the sub control volume to the nodes. These interpolated values are used in the shape function derivative loop to calculate the second derivatives.

  The default is to include the source term while the specification of it is placed as a temporary field, i.e., can be changed as restart.

###### Omit Near Wall Turbulent Ke Transport Equation

Syntax

  Omit Near Wall Turbulent Ke Transport Equation

Summary

  Do not construct a transport equation for the near wall turbulent kinetic energy equation.

Description

  Rather than solving a transport equation for the near wall turbulent transport equation, assign a Dirichlet condition based on local equilibrium argument between production and dissipation that yields . This formulation neglects convection and diffusion effects for the near wall equation.

###### Omit Turbulence Source Terms On Block(S)

Syntax

  Omit Turbulence Source Terms On Block(S) BlockList…

Summary

  Omit source terms on these sets of I/O block; specified by name.

Description

  This line command will result in all turbulence source terms to be zeroed in the respective blocks. We can not yet dial in exact equation sets. Example usage: OMIT TURBULENCE SOURCE TERMS ON BLOCK(S) block_1 block_2.

  Note that the source terms for output will still exist and, in general, be non-zero within the skipped block. However, the contribution to the equation system will be omitted.

Parameter | Value | Default
--- | --- | ---
BlockList | string… | –

###### Omit Velocity Divergence In Turbulent Production Term

Syntax

  Omit Velocity Divergence In Turbulent Production Term

Summary

  Do not include divergence term in turbulence production

Description

  This option removes the divergence term from the turbulent production of kinetic energy. The default is to include this term.

###### Time Filter

Syntax

  Time Filter {=} Value

Summary

  Time filter size for Time Filtered Navier-Stokes model

Description

  Turbulent viscosity is normally calculated based on a time scale given by k/epsilon (for k-epsilon models) or T (v2f model). The TFNS model substitutes the minimum of the normal computed value and the user-specified time filter size in the turbulent viscosity calculation. In general, this filter should be no less than twice the physical time step. A non-fatal warning is issued if this condition is violated. (Default: 1.0e32 to essentially deactivate the model)

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Value | real | 1.0e32

###### Turbulence Model

Syntax

  Turbulence Model {=} {dksgs | dsmag | inagaki_ksgs | ke | ksgs | kw | lam | lrke | lrkw | lrsst | rng | smag | sst | sstdes | v2f}

Summary

  Specify type of turbulence model to be used

Description

  Fuego provides a broad set of turbulence models which includes both RANS and LES models. For more information regarding specific models, please see the theory documentation. One note of importance is that the SST, SSTDES, and LRSST models require the `min_wall_distance` field, which is a measure of the nearest distance to a wall. Fuego will automatically use Sierra/Krino library to generate this field when using these turbulence models.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
TurbModel | {dksgs | dsmag | inagaki_ksgs | ke | ksgs | kw | lam | lrke | lrkw | lrsst | rng | smag | sst | sstdes | v2f} | LAM

###### Turbulence Model Parameter

Syntax

  Turbulence Model Parameter {frequency_scaling | kappa | minimum_k | yplus_crit} {=} Value

Summary

  Specify turbulence model parameters

Parameter | Value | Default
--- | --- | ---
TurbulenceModelParams | {frequency_scaling | kappa | minimum_k | yplus_crit} | –
{=} | {= | are | is} | –
Value | real | –

###### Turbulence Postprocessor

Syntax

  Turbulence Postprocessor {=} {q_criterion | residual_reynolds_stress | resolved_reynolds_stress}

Summary

  Specify a turbulence postprocessor

Description

  A set of post processors for turbulence quantities. Options include RESOLVED_REYNOLDS_STRESS, RESIDUAL_REYNOLDS_STRESS, and Q_CRITERION.

  warning{The RESOLVED_REYNOLDS_STRESS and RESIDUAL_REYNOLDS_STRESS options are deprecated and should be replaced with the appropriate post-processor in the averaging block.}

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
TurbPP | {q_criterion | residual_reynolds_stress | resolved_reynolds_stress} | RESOLVED_REYNOLDS_STRESS

###### Under Relax Turbulent_Viscosity By

Syntax

  Under Relax Turbulent_Viscosity By Urf

Summary

  Under relaxation factor for the turbulent viscosity

Parameter | Value | Default
--- | --- | ---
Urf | real | –

###### Use Buoyant Vorticity Generation

Syntax

  Use Buoyant Vorticity Generation At Value Seconds

Summary

  Use the BVG model of Nicollete and Tieszen

Description

  Invoke the buoyant vorticity generation augmentation to the turbulent kinetic energy production term. Allow for a delay in the activation to avoid potential instabilities. The delay will will be only in assembling the source term to the appropriate partial differential equation. However, the source term will be computed at all times when the model is activated, and will be limited to a fraction of the dissipation rate.

  This model has not been validated for use in the context of turbulence models other than the standard - model. The model uses the turbulence model parameters and .

Parameter | Value | Default
--- | --- | ---
Value | real | –

###### Use Dynamic Ksgs

Syntax

  Use Dynamic Ksgs

Summary

  Compute model coefficients dynamically for KSGS turbulent model

Description

  warning{This command is deprecated. Use the DKSGS turbulence model to activate this.}

###### Wall Distance Band Size

Syntax

  Wall Distance Band Size {=} BandSize

Summary

  Band size for the normal distance to the wall calculation. Set to 10x the max face element size if omitted.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
BandSize | real | –

###### Wall Model

Syntax

  Wall Model {=} {modeled | resolved}

Summary

  Specify wall model to be used

Description

  Options are MODELED and RESOLVED; intended for LES usage. Current default depends on which turbulence model is in use. For Smagorinsky LES, the wall value for wall shear stress must be based on a nonlinear iteration for the wall friction velocity, or “DETERMINE UTAU VIA NONLINEAR LAW OF THE WALL ITERATION”.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
WallModel | {modeled | resolved} | –

## 7.7.16. Acoustic Transfer Output

Scope

  Solution Options

Summary

  Specify transfer output of the divergence of the Lighthill tensor to a different mesh for use in acoustic simulations.

    begin Acoustic Transfer Output DefinitionName

       At Step n {increment | interval} {=} m

       At Time Dt1 {increment | interval} {=} Dt2

       Force Search In Model Coordinates

       Input Mesh Name {=} MeshName

       Output Mesh Name {=} MeshName

       Overlap Drop Tolerance {=} DropTol

       Send Block From_blocks... To To_blocks...

       Source Vector Name {=} SrcName [ Scaling {=} ScalingValue  ]

       Timestep Adjustment Interval {=} Nsteps

    end Acoustic Transfer Output DefinitionName

### 7.7.16.1. Line Commands

###### At Step

Syntax

  At Step n {increment | interval} {=} m

Summary

  Specify an output interval in terms of the internal iteration step count. The first step specifies the step count at the beginning of this interval and the second step specifies the output frequency to be used within this interval.

Parameter | Value | Default
--- | --- | ---
n | integer | –
Option | {increment | interval} | –
{=} | {= | are | is} | –
m | integer | –

###### At Time

Syntax

  At Time Dt1 {increment | interval} {=} Dt2

Summary

  Specify an output interval in terms of the internal simulation time. The first time specifies the time at the beginning of this time interval and the second time specifies the output frequency to be used within this interval.

Parameter | Value | Default
--- | --- | ---
Dt1 | real | –
Option | {increment | interval} | –
{=} | {= | are | is} | –
Dt2 | real | –

###### Force Search In Model Coordinates

Syntax

  Force Search In Model Coordinates

Summary

  By default the geometric search will be repeated in the current coordinates at each time step for problems with mesh motion. Adding this line command will force the search to be done once at the start of the problem in the model coordinates.

###### Input Mesh Name

Syntax

  Input Mesh Name {=} MeshName

Summary

  Specify the input mesh that will be the destination of the transfer.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
MeshName | string | –

###### Output Mesh Name

Syntax

  Output Mesh Name {=} MeshName

Summary

  Specify where to output the result of the transfer.

Description

  The divergence of the Lighthill tensor will be output as divT

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
MeshName | string | –

###### Overlap Drop Tolerance

Syntax

  Overlap Drop Tolerance {=} DropTol

Summary

  Specify an overlap drop tolerance.

Description

  Specify a volume fraction to ignore overlaps below. This does not affect conservation, if you set a tolerance of 5% (0.05) and a fluid element overlaps with one acoustic element by 97% and the remaining 3% with other elements, then 100% of the source term would be sent to the single acoustic element. This can reduce the cost and memory use of the acoustic transfer.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
DropTol | real | –

###### Send Block

Syntax

  Send Block From_blocks… To To_blocks…

Summary

  The acoustic transfer will define one transfer operation per SEND BLOCK line, but can define many from/to blocks per line. If there is a block with mesh motion in the send block list it will update that transfer every time step unless you have forced the search to be done in model coordinates. If you have some moving blocks and some fixed blocks it may be faster to split the moving block into its own transfer as long as this is geometrically reasonable.

      SEND BLOCK block_3 block_5 block_6 TO block_3 block_5
      SEND BLOCK block_7 TO block_1

Parameter | Value | Default
--- | --- | ---
From_blocks | string… | –
To_blocks | string… | –

###### Source Vector Name

Syntax

  Source Vector Name {=} SrcName [ Scaling {=} ScalingValue ]

Summary

  Specify the noise source vector name.

Description

  The divergence of the Lighthill tensor will be output as divT. This specifies the name of the source vector to transfer. By default this is “div_lighthill_tensor” but if you are using a filter or averaging you should set the name here to the name of the filtered vector.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
SrcName | string | –

###### Timestep Adjustment Interval

Syntax

  Timestep Adjustment Interval {=} Nsteps

Summary

  Specify the number of steps to ‘look ahead’ and adjust the timestep to ensure that the specified output times or simulation end time will be hit ‘exactly’.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Nsteps | integer | –

## 7.7.17. Point Source

Scope

  Solution Options

Summary

  Specify a point source.

    begin Point Source DefinitionName

        {contact_angle | edc_product | gas_volume_fraction | mixture_fraction | pressure | progress_variable | scalar_variance | second_mixture_fraction | solid_volume_fraction | soot_mass_fraction | soot_nuclei_mass_fraction | temperature | turbulent_dissipation | turbulent_frequency | turbulent_helmholtz_function | turbulent_kinetic_energy | turbulent_v2 | volume_of_fluid | x_solid_velocity | x_velocity | y_solid_velocity | y_velocity | z_solid_velocity | z_velocity} {=} Value

       Location {=} {node nearest | sphere at} Location1 Location2 Location3 [ Radius {=} RadiusValue  ]

       Mdot {=} Mdot

       Mass_Fraction Species {=} Mass fraction

       Progress_Variable ProgressVariableName {=} Value

    end Point Source DefinitionName

### 7.7.17.1. Line Commands

###### Primitivevariable

Syntax

  Primitivevariable {contact_angle | edc_product | gas_volume_fraction | mixture_fraction | pressure | progress_variable | scalar_variance | second_mixture_fraction | solid_volume_fraction | soot_mass_fraction | soot_nuclei_mass_fraction | temperature | turbulent_dissipation | turbulent_frequency | turbulent_helmholtz_function | turbulent_kinetic_energy | turbulent_v2 | volume_of_fluid | x_solid_velocity | x_velocity | y_solid_velocity | y_velocity | z_solid_velocity | z_velocity} {=} Value

Summary

  Assign inflow condition to the specified variable. Specified value can be a constant or a string function of time or global variables. Omitted properties will default to the reference value, and if no reference value is present will default to 0.

Parameter | Value | Default
--- | --- | ---
PrimitiveVariable | {contact_angle | edc_product | gas_volume_fraction | mixture_fraction | pressure | progress_variable | scalar_variance | second_mixture_fraction | solid_volume_fraction | soot_mass_fraction | soot_nuclei_mass_fraction | temperature | turbulent_dissipation | turbulent_frequency | turbulent_helmholtz_function | turbulent_kinetic_energy | turbulent_v2 | volume_of_fluid | x_solid_velocity | x_velocity | y_solid_velocity | y_velocity | z_solid_velocity | z_velocity} | –
{=} | {= | are | is} | –
Value | “string” | –

###### Location

Syntax

  Location {=} {node nearest | sphere at} Location1 Location2 Location3 [ Radius {=} RadiusValue ]

Summary

  Specify the location of the point source. The source will be applied at the node closest to the specified location. If mesh motion is active, the node will be selected only once at the initial mesh coordinates.

  The source location can either be the node nearest to a point, or a sphere where the source is applied evenly on all enclosed nodes. If the sphere does not intersect any nodes, the closest node is used.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
LocationType | {node nearest | sphere at} | –
Location | real1 real2 real3 | –

###### Mdot

Syntax

  Mdot {=} Mdot

Summary

  Specify the mass flow rate of the point source. Can be a constant or string function of time and global variables. This should be in mass/time units (e.g. kg/s). Positive (inflow) and negative (outflow) values are both allowed.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Mdot | “string” | –

###### Mass_Fraction

Syntax

  Mass_Fraction Species {=} Mass fraction

Summary

  Set the source mass fraction. Specified value can be a constant or a string function of time or global variables. Omitted mass fractions will default to 0.

Parameter | Value | Default
--- | --- | ---
Species | string | –
{=} | {= | are | is} | –
Mass fraction | “string” | –

###### Progress_Variable

Syntax

  Progress_Variable ProgressVariableName {=} Value

Summary

  Set the source progress variable. Specified value can be a constant or a string function of time or global variables.

Parameter | Value | Default
--- | --- | ---
ProgressVariableName | string | –
{=} | {= | are | is} | –
Value | “string” | –

## 7.7.18. Mesh Motion Specification

Scope

  Solution Options

Summary

  Specify mesh motion parameters.

    begin Mesh Motion Specification DefinitionName

       Activate Bdf2 For Mesh Velocity

       Mesh Motion Model On BlockName {=} {fixed_const_velocity | none | rigid_body | rotation | specified | transferred} [ DisplacementArgs...  ]

       begin Rigid Body Motion Model DefinitionName
       end

    end Mesh Motion Specification DefinitionName

### 7.7.18.1. Line Commands

###### Activate Bdf2 For Mesh Velocity

Syntax

  Activate Bdf2 For Mesh Velocity

Summary

  Activation of the second-order BDF2 time integrator for mesh velocity.

Description

  BDF2 is a A-stable, three state time integrator that has been demonstrated to be well performing in the low-Mach application space. When activated, the mesh velocity calculated from displacements will use BDF2. This is enabled automatically if the overall time integration is set to use BDF2.

###### Mesh Motion Model On

Syntax

  Mesh Motion Model On BlockName {=} {fixed_const_velocity | none | rigid_body | rotation | specified | transferred} [ DisplacementArgs… ]

Summary

  Specify the mesh motion model to use.

Description

  Select the mesh motion model (SPECIFIED, FIXED_CONST_VELOCITY, TRANSFERRED, ROTATION, or NONE) along with any additional model arguments.

  The ‘SPECIFIED’ model takes either a set of specified displacements that are string functions of t, x, y, and z, or a specified set of accelerations that are functions of t and any global variables. In the latter mode, an initial velocity, v0, can also be specified (default: 0).

  The ‘TRANSFERRED’ and ‘NONE’ options do not take any arguments.

  The ‘FIXED_CONST_VELOCITY’ lets you apply motion to a block without actually moving it in the model. This is typically applied to shells, for example to move the top fluid in a lid-driven cavity flow without actually moving the mesh, or to apply motion on a quarter of a circle without actually moving it.

  The ‘ROTATION’ model takes a time function for the angle (theta) in rotations (radius/2*pi or degrees/360), and an origin and rotation axis (only for 3D). For example, a rotation of 1 rpm would use ‘theta=t/60’. The rotation uses the right hand rule about the specified axis and origin. Rotation can also be specified by providing an angular acceleration term that can be a function of time (t) or global variables. An optional initial angular velocity (omega0) can also be specified (default: 0). Both the angular acceleration and angular velocity are specified in revolutions, so they are multiplied internally by 2*pi to convert to radians.

  Any blocks that don’t have a mesh motion model specified get no displacement. Some example syntax is shown below. You can use the “all_blocks” keyword to specify all blocks, but it cannot be mixed with per-block specifications.

      MESH MOTION MODEL ON block_1    = SPECIFIED D = 0.1*t y*z sin(t)
      MESH MOTION MODEL ON block_1    = SPECIFIED v0 = 0.1 0 0 a=0 0.1 0
      MESH MOTION MODEL ON all_blocks = TRANSFERRED
      MESH MOTION MODEL ON block_3    = ROTATION  origin=0 0 0 \$
          axis=1 0 0 theta=t/60
      MESH MOTION MODEL ON block_3    = ROTATION  origin=0 0 0 \$
          axis=1 0 0 omega0=1/60 alpha=0
      MESH MOTION MODEL ON block_4    = NONE
      MESH MOTION MODEL ON block_6    = FIXED_CONST_VELOCITY \$
          Velocity=0.1 0*t "0 + 4*x*y"

  The mesh motion model also generates global variables of its internal state (position, velocity, and acceleration) which can be used in the functional forms. These global variables are output in units of revolutions for consistency with the input units. For example, to smoothly accelerate up to a constant angular velocity of 10 rev/s, you could use:

      MESH MOTION MODEL ON block_3 = ROTATION  origin=0 0 0 \$
          axis=1 0 0 alpha=10-block_3_omega

Parameter | Value | Default
--- | --- | ---
BlockName | string | –
{=} | {= | are | is} | –
MeshMotionModel | {fixed_const_velocity | none | rigid_body | rotation | specified | transferred} | –

## 7.7.19. Rigid Body Motion Model

Scope

  Mesh Motion Specification

Summary

  Specify parameters for 6-DOF rigid body motion.

    begin Rigid Body Motion Model DefinitionName

       Acceleration {=} Acceleration1 Acceleration2 Acceleration3

       Blocks {=} BlockNames...

       Buoyant Object Mass {=} ObjectMass...

       Buoyant Object Pitch Moment {=} Moment

       Buoyant Object Roll Moment {=} Moment

       Buoyant Object Surfaces {=} ObjSurfaces...

       Buoyant Object Yaw Moment {=} Moment

       Initial Velocity {=} InitialVelocity1 InitialVelocity2 InitialVelocity3

       Origin {=} OriginCoords1 OriginCoords2 OriginCoords3

       Pitch Acceleration {=} PitchAcceleration

       Pitch Initial Velocity {=} PitchInitialVelocity

       Roll Acceleration {=} RollAcceleration

       Roll Axis {=} RollAxis1 RollAxis2 RollAxis3

       Roll Initial Velocity {=} RollInitialVelocity

       Under Relaxation {=} UnderRelaxation

       Yaw Acceleration {=} YawAcceleration

       Yaw Axis {=} YawAxis1 YawAxis2 YawAxis3

       Yaw Initial Velocity {=} YawInitialVelocity

    end Rigid Body Motion Model DefinitionName

### 7.7.19.1. Line Commands

###### Acceleration

Syntax

  Acceleration {=} Acceleration1 Acceleration2 Acceleration3

Summary

  Specify the translational acceleration

Description

  Specify the translational acceleration using three quoted string functions. Functions can include time and any global variables as valid variables.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Acceleration | “string”1 “string”2 “string”3 | –

###### Blocks

Syntax

  Blocks {=} BlockNames…

Summary

  Specify which blocks to apply this model to.

Description

  Give a list of blocks to apply the model to. The all_blocks command is permitted here too.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
BlockNames | string… | –

###### Buoyant Object Mass

Syntax

  Buoyant Object Mass {=} ObjectMass…

Summary

  Specify the buoyant object mass

Description

  Specify the buoyant object mass. Optionally, you can specify three values for mass to act on the three translation directions. This is primarily useful for suppressing motion in a given direction by setting that mass to a very large number. For example, to only allow motion of a 50 kg object in the z-direction you could set the mass to:

      BUOYANT OBJECT MASS = 1e30 1e30 50

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
ObjectMass | real… | –

###### Buoyant Object Pitch Moment

Syntax

  Buoyant Object Pitch Moment {=} Moment

Summary

  Specify the buoyant object pitch moment

Description

  Specify the buoyant object moment of inertia about pitch axis. Set to a very large number to disable pitch.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Moment | real | –

###### Buoyant Object Roll Moment

Syntax

  Buoyant Object Roll Moment {=} Moment

Summary

  Specify the buoyant object roll moment

Description

  Specify the buoyant object moment of inertia about roll axis. Set to a very large number to disable roll.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Moment | real | –

###### Buoyant Object Surfaces

Syntax

  Buoyant Object Surfaces {=} ObjSurfaces…

Summary

  Specify surfaces of a buoyant object.

Description

  Specify surfaces of a buoyant object.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
ObjSurfaces | string… | –

###### Buoyant Object Yaw Moment

Syntax

  Buoyant Object Yaw Moment {=} Moment

Summary

  Specify the buoyant object yaw moment

Description

  Specify the buoyant object moment of inertia about yaw axis. Set to a very large number to disable yaw.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
Moment | real | –

###### Initial Velocity

Syntax

  Initial Velocity {=} InitialVelocity1 InitialVelocity2 InitialVelocity3

Summary

  Specify the translational initial velocity

Description

  Specify the translational initial velocity using three quoted string functions. Functions can include time and any global variables as valid variables.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
InitialVelocity | “string”1 “string”2 “string”3 | –

###### Origin

Syntax

  Origin {=} OriginCoords1 OriginCoords2 OriginCoords3

Summary

  Specify the origin for the motion.

Description

  The origin coordinates are those around which rotation occurs. This would typically be the center of mass.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
OriginCoords | real1 real2 real3 | –

###### Pitch Acceleration

Syntax

  Pitch Acceleration {=} PitchAcceleration

Summary

  Specify the pitch acceleration

Description

  Specify the pitch acceleration using a quoted string function. Functions can include time and any global variables as valid variables. Units are revolutions, not radians.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
PitchAcceleration | “string” | –

###### Pitch Initial Velocity

Syntax

  Pitch Initial Velocity {=} PitchInitialVelocity

Summary

  Specify the pitch initial velocity

Description

  Specify the pitch initial velocity using a quoted string function. Functions can include time and any global variables as valid variables. Units are revolutions, not radians.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
PitchInitialVelocity | “string” | –

###### Roll Acceleration

Syntax

  Roll Acceleration {=} RollAcceleration

Summary

  Specify the roll acceleration

Description

  Specify the roll acceleration using a quoted string function. Functions can include time and any global variables as valid variables. Units are revolutions, not radians.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
RollAcceleration | “string” | –

###### Roll Axis

Syntax

  Roll Axis {=} RollAxis1 RollAxis2 RollAxis3

Summary

  Specify the roll axis for rotation.

Description

  Rotation is specified using pitch, roll, and yaw.

  Roll is rotation about the roll axis. Yaw is rotation about the yaw axis. The pitch axis is defined by the cross product of the roll and yaw axes.

  Rotation is applied as roll, then pitch, then yaw. The axes about which these translations happen are fixed.

  The roll and yaw axes must be orthogonal. These do not need to be unit vectors, they will be normalized internally.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
RollAxis | real1 real2 real3 | –

###### Roll Initial Velocity

Syntax

  Roll Initial Velocity {=} RollInitialVelocity

Summary

  Specify the roll initial velocity

Description

  Specify the roll initial velocity using a quoted string function. Functions can include time and any global variables as valid variables. Units are revolutions, not radians.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
RollInitialVelocity | “string” | –

###### Under Relaxation

Syntax

  Under Relaxation {=} UnderRelaxation

Summary

  Specify under-relaxation for the equations of motion

Description

  Specify under-relaxation for the equations of motion

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
UnderRelaxation | real | 1

###### Yaw Acceleration

Syntax

  Yaw Acceleration {=} YawAcceleration

Summary

  Specify the yaw acceleration

Description

  Specify the yaw acceleration using a quoted string function. Functions can include time and any global variables as valid variables. Units are revolutions, not radians.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
YawAcceleration | “string” | –

###### Yaw Axis

Syntax

  Yaw Axis {=} YawAxis1 YawAxis2 YawAxis3

Summary

  Specify the yaw axis for rotation.

Description

  Rotation is specified using pitch, roll, and yaw.

  Roll is rotation about the roll axis. Yaw is rotation about the yaw axis. The pitch axis is defined by the cross product of the roll and yaw axes.

  Rotation is applied as roll, then pitch, then yaw. The axes about which these translations happen are fixed.

  The roll and yaw axes must be orthogonal. These do not need to be unit vectors, they will be normalized internally.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
YawAxis | real1 real2 real3 | –

###### Yaw Initial Velocity

Syntax

  Yaw Initial Velocity {=} YawInitialVelocity

Summary

  Specify the yaw initial velocity

Description

  Specify the yaw initial velocity using a quoted string function. Functions can include time and any global variables as valid variables. Units are revolutions, not radians.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
YawInitialVelocity | “string” | –

## 7.7.20. Vof Model Specification

Scope

  Solution Options

Summary

  Specify a number of physical parameters that are to be used for multi-phase VOF flow simulations.

    begin Vof Model Specification DefinitionName

       Interface Compression Factor {=} VOFInterfaceCompressionFactor

       Interface Compression Model {=} {adaptive | constant | none}

       Interface Curvature Algorithm {=} {diffusive | level_set | none}

       Interface Location Tolerance {=} InterfaceTol

       Interface Sharpening Model {=} {non_conserving | none | volume_conserving}

       Num Smoother Iterations {=} NumSmootherIters

       Phase Change Model {=} {constant | langmuir | none | thermal} [ModelArgs]...

       Post Process Interface Normal

       Smoother Fourier Number {=} SmootherFo

    end Vof Model Specification DefinitionName

### 7.7.20.1. Line Commands

###### Interface Compression Factor

Syntax

  Interface Compression Factor {=} VOFInterfaceCompressionFactor

Summary

  Specify parameters for interface compression model for VOF.

Description

  Select the VOF interface compression factor (only used in the Constant model)

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
VOFInterfaceCompressionFactor | real | –

###### Interface Compression Model

Syntax

  Interface Compression Model {=} {adaptive | constant | none}

Summary

  Specify parameters for interface compression model for VOF.

Description

  Select the VOF interface compression model (Constant, Adaptive, or None)

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
VOFInterfaceCompressionModel | {adaptive | constant | none} | –

###### Interface Curvature Algorithm

Syntax

  Interface Curvature Algorithm {=} {diffusive | level_set | none}

Summary

  Specify the curvature model to use.

Description

  Select the VOF curvature model (DIFFUSIVE, LEVEL_SET, or NONE)

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
VOFSmootherAlgorithm | {diffusive | level_set | none} | –

###### Interface Location Tolerance

Syntax

  Interface Location Tolerance {=} InterfaceTol

Summary

  Specify parameters for interface location for VOF.

Description

  Select the tolerance used to identify the interface zone

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
InterfaceTol | real | –

###### Interface Sharpening Model

Syntax

  Interface Sharpening Model {=} {non_conserving | none | volume_conserving}

Summary

  Specify parameters for interface sharpening model for VOF.

Description

  Select the VOF interface sharpening model (Volume_Conserving or None)

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
VOFInterfaceSharpeningModel | {non_conserving | none | volume_conserving} | –

###### Num Smoother Iterations

Syntax

  Num Smoother Iterations {=} NumSmootherIters

Summary

  Specify parameters for interface smoothing for VOF.

Description

  Select the number of smoother iterations for the interface normal calculation

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
NumSmootherIters | integer | –

###### Phase Change Model

Syntax

  Phase Change Model {=} {constant | langmuir | none | thermal} [ModelArgs]…

Summary

  Specify the phase change model to use.

Description

  Select the VOF phase change model (CONSTANT, THERMAL, or NONE)

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
VOFPhaseChangeModel | {constant | langmuir | none | thermal} | –
ModelArgs | [string]… | –

###### Post Process Interface Normal

Syntax

  Post Process Interface Normal

Summary

  Post-process the interface normal vector

###### Smoother Fourier Number

Syntax

  Smoother Fourier Number {=} SmootherFo

Summary

  Specify parameters for interface smoothing for VOF.

Description

  Select the Fourier number for the interface diffusive smoother

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
SmootherFo | real | –

## 7.7.21. Postprocess

Scope

  Fuego Region

Summary

  Defines a custom post-processor block to be run at the end of the time step.

Description

  The block type defines the post-processor operation performed, as in:

      Begin postprocess Integral

  or

      Begin postprocess Average

  The valid types are described below.

  Integral

  Perform an integral of the specified scalar function () on either the specified volume (blocks) or surface (sidesets) and save the result as a global variable. The function can depend on time and space (,,,) and any nodal variable.

  On volumes this is:

  while on surfaces it is:

  Average

  Perform a volume or area weighted average of the specified scalar function () on either the specified volume (blocks) or surface (sidesets) and save the result as a global variable. The function can depend on time and space (,,,) and any nodal variable.

  On volumes this is:

  while on surfaces it is:

  Sum

  Find the nodal summation of the specified scalar function () on either the specified volume (blocks) or surface (sidesets) and save the result as a global variable. The function can depend on time and space (,,,) and any nodal variable.

  Min

  Find the nodal minimum of the specified scalar function () on either the specified volume (blocks) or surface (sidesets) and save the result as a global variable. The function can depend on time and space (,,,) and any nodal variable.

  Max

  Find the nodal maximum of the specified scalar function () on either the specified volume (blocks) or surface (sidesets) and save the result as a global variable. The function can depend on time and space (,,,) and any nodal variable.

  L2_Norm

  Find the nodal L2-norm of the specified scalar function () on either the specified volume (blocks) or surface (sidesets) and save the result as a global variable. The function can depend on time and space (,,,) and any nodal variable.

  On volumes this is:

  while on surfaces it is:

  Global

  Evaluate a global function () and save the result as a global variable. The function can depend on time and any other global variable. You should not specify any location entries for a global post-processor.

      Begin postprocess Global
        Output name = maxTempC
        Function = "maxTemp - 273.15"
      End

  Nodal_Field

  Evaluate the specified scalar function () on either the specified volume (blocks) or surface (sidesets) and save the result in a nodal field. The function can depend on time and space (,,,) and any nodal variable.

      Begin postprocess Nodal_Field
        Output name = nuCalc
        Location = all_blocks
        Function = "viscosity/density"
      End

  Integrated_Flux

  Evaluate the integrated flux of a specified vector function (requires 2 or 3 components for depending on problem dimension). This must be performed on surfaces, not on volumes. The result is saved in a global variable. The functions can depend on time and space (,,,) and any nodal variable.

      Begin postprocess Integrated_Flux
        Output name = mass_flux
        Location = surface_1
        Function = "density*x_velocity" \$
                   "density*y_velocity" \$
                   "density*z_velocity"
      End

  Point

  Evaluate the specified function at a specific point in space and save the result as a global variable. The location to query should be specified as 2 or 3 coordinates in the Location command. If the specified coordinates lie outside all the mesh elements an error will be thrown. The functions can depend on time and space (,,,) and any nodal variable.

      Begin postprocess Point
        Output name = TC1
        Location = 1.2 2.2 0.1
        Function = "temperature"
      End

    begin Postprocess

       Evaluation Time {=} {after_fluid | after_pmr}

       Function {=} FunctionStr...

       Location {=} MeshEntites...

       Output Name {=} OutputName

    end Postprocess

### 7.7.21.1. Line Commands

###### Evaluation Time

Syntax

  Evaluation Time {=} {after_fluid | after_pmr}

Summary

  Define whether to execute the utility after the fluid solve or after the PMR solve. Default behavior is to run after the PMR solve. If the post-processed quantity uses PMR fields, one may want to run them with the same values as were used in the fluid solve (After_Fluid) or with the updated values returned from the PMR solve (After_PMR).

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
PPEvalTime | {after_fluid | after_pmr} | After_PMR

###### Function

Syntax

  Function {=} FunctionStr…

Summary

  Provide a string function to evaluate in the post-processor.

Description

  A quoted function string for the post-processor to evaluate. For the FLUX post-processor you must provide multiple quoted entries - one per spatial dimension. For all other types you may only provide a single function string.

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
FunctionStr | “string”… | –

###### Location

Syntax

  Location {=} MeshEntites…

Summary

  Mesh locations to evaluate the post-processor at.

Description

  A list of block or sideset names to evaluate the post-processor at. For multiple blocks you can either include them all in one line or add separate lines. The aliases “all_blocks” and “all_surfaces” can also be used. You cannot mix blocks and sidesets in a single post-processor block.

      Begin postprocess nodal_field
        Output name = nuCalc
        Location = all_blocks
        Function = "viscosity/density"
      End

      Begin postprocess nodal_field
        Output name = nuCalc
        Location = block_1 block_2 block_3
        Function = "viscosity/density"
      End

      Begin postprocess nodal_field
        Output name = nuCalc
        Location = block_1
        Location = block_2
        Location = block_3
        Function = "viscosity/density"
      End

  When using the “POINT” operation the location command should be the coordinates to evaluate the function at.

      Begin postprocess point
        Output name = TC1
        Location = 1.2 2.2 0.1
        Function = "temperature"
      End

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
MeshEntites | string… | –

###### Output Name

Syntax

  Output Name {=} OutputName

Summary

  Define the name for the output variable (global or nodal depending on the type).

Parameter | Value | Default
--- | --- | ---
{=} | {= | are | is} | –
OutputName | string | –