7.7. Fuego Region

This section is referenced in the following other sections

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

   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

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.

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 $T^4$ and $T_{\mathrm{ref}}^4$ to approximate radiation to the far field.
Description: Calculates the scalar_flux term as $4 * \epsilon * \sigma * T_{\mathrm{ref}}^4$ 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:

$\bar\phi = \frac{1}{T} \int \phi(t)\, dt$

where $\phi(t)$ is the quantity of interest at time $t$ and the integration is over $(0,T)$ , the time interval which is averaged.

The Favre average is the ratio of two Reynolds averages:

$\tilde\phi = \frac{\bar{\rho\phi}}{\bar\rho}$

Where $\phi$ 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 $1.0e-5$ 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 $1.0e-5$ the filter will be valid. If the analysis time step drops below $1.0e-5$ 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

$\overline{S_{ij}} = \overline{\rho}\overline{u^\prime_i u^\prime_j} = \overline{\rho} \left(\overline{u_i u_j} - \bar{u_i} \bar{u_j} \right)$

RESOLVED_FAVRE_STRESS

$\widetilde{S_{ij}} = \overline{\rho}\widetilde{u^{\prime\prime}_i u^{\prime\prime}_j} = \overline{\rho} \left(\widetilde{u_i u_j} - \widetilde{u_i} \widetilde{u_j} \right)$

RESOLVED_TURBULENT_KINETIC_ENERGY

$\widetilde{k} = \frac{1}{2} \widetilde{u^{\prime\prime}_k u^{\prime\prime}_k}$

RESOLVED_PRODUCTION

$\widetilde{P_k} = -\widetilde{S_{ij}} \frac{\partial \widetilde{u}_i}{\partial x_j}$

RESOLVED_DISSIPATION

$\widetilde{\epsilon} = \frac{1}{\overline{\rho}} \overline{2 \mu S^{\prime\prime}_{ij} \frac{\partial u^{\prime\prime}_{i}}{\partial x_j}}$

$S^{\prime\prime}_{ij} = \frac{1}{2} \left( \frac{\partial u^{\prime\prime}_i}{\partial x_j} + \frac{\partial u^{\prime\prime}_j}{\partial x_i} \right) - \frac{1}{3} \frac{\partial u^{\prime\prime}_k}{\partial x_k} \delta_{ij}$

RESOLVED_SCALAR_FLUX

$\widetilde{F_{\phi}} = \overline{\rho} \left( \widetilde{u_i \phi} - \widetilde{u_i} \widetilde{\phi} \right)$

MODELED_REYNOLDS_STRESS

$\widetilde{S_{ij}} = -2 \mu^t \widetilde{S}^*_{ij}$

$\widetilde{S}^*_{ij} = \frac{1}{2} \left( \frac{ \partial \widetilde{u}_i}{\partial x_j} + \frac{ \partial \widetilde{u}_j}{ \partial x_i}\right)$

MODELED_SCALAR_FLUX

$\widetilde{F_{\phi}} = -\frac{\mu^t}{\mathrm{Pr^t}} \frac{\partial \widetilde{\phi}}{\partial x_i}$

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:

$\tilde\phi = \frac{\bar{\rho\phi}}{\bar\rho}$

Where $\phi$ is the quantity of interest and $\rho$ 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, $\bar{\rho\phi}$ , 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 ( $A$ ) using the source field ( $S$ ) and a blending coefficient ( $\alpha$ ):

$\alpha = min\left(1, \frac{\Delta t}{t_{filt}}\right)$

$A = (1 - \alpha) A + \alpha S$

The filter time ( $t_{filt}$ ) 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:

$\bar\phi = \frac{1}{T} \int \phi(t)\, dt$

where $\phi(t)$ is the quantity of interest at time $t$ and the integral is evaluated over $(0,T)$ , 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, $\bar{\rho\phi}$ , 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 $(T_0 + nT, T_0 (n+1)T)$ where $T_0$ 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 $T$ , The Reynolds or Favre averages specified will be determined over intervals of length $T$ . The intervals will be over $(nT, (n+1)T)$ for integers $n$ . 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 $(T_0 + nT, T_0 (n+1rT)$ where $T_0$ 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

   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	–

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...  ]

   Edge Variables {=} [ VariableList...  ]

   Element [ VariableList...  ]

   Element Variables {=} [ VariableList...  ]

   Enable Large Ids

   Exclude {=} [ ElementBlockList...  ]

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

   Face [ VariableList...  ]

   Face Variables {=} [ VariableList...  ]

   Flush Interval {=} Option

   Global [ Variables...  ]

   Global Variables {=} [ Variables...  ]

   Include {=} [ ElementBlockList...  ]

   Nodal [ VariableList...  ]

   Nodal Variables {=} [ VariableList...  ]

   Node [ VariableList...  ]

   Node Variables {=} [ VariableList...  ]

   Nodeset [ VariableList...  ]

   Nodeset Variables {=} [ 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...  ]

   Sideset Variables {=} [ VariableList...  ]

   Start Time {=} Start_time

   Surface [ VariableList...  ]

   Surface Variables {=} [ 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.

Edge Variables

Syntax: Edge Variables {=} [ 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
{=}	{= \| are \| is}	–

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”

Element Variables

Syntax: Element Variables {=} [ 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
{=}	{= \| are \| is}	–

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.

Face Variables

Syntax: Face Variables {=} [ 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
{=}	{= \| are \| is}	–

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 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.

Global Variables

Syntax: Global Variables {=} [ Variables… ]
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
{=}	{= \| are \| is}	–

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.

Nodal Variables

Syntax: Nodal Variables {=} [ 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
{=}	{= \| are \| is}	–

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.

Node Variables

Syntax: Node Variables {=} [ 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
{=}	{= \| are \| is}	–

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.

Nodeset Variables

Syntax: Nodeset Variables {=} [ 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
{=}	{= \| are \| is}	–

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.

Sideset Variables

Syntax: Sideset Variables {=} [ 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
{=}	{= \| are \| is}	–

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.

Surface Variables

Syntax: Surface Variables {=} [ 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
{=}	{= \| are \| is}	–

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, $\frac{\partial p}{\partial t} + u_j \frac{\partial p}{\partial x_j}$ , to the laminar or turbulent enthalpy transport equation and to the laminar temperature transport equation. Additionally, the viscous work term $u_i \frac{\partial \tau_{ij}}{\partial x_j}$ 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:

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, $0 \lt x \lt 1$

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

BLENDING uses HYBRID UPWIND FACTOR ( $\zeta$ ) and the function is, $\chi = \frac{(\zeta Pe)^2}{5+(\zeta Pe)^2}$ .

TAHH follows hyperbolic tangent profile between $\chi$ and Pe. It uses shift p (HYBRID UPWIND SHIFT) and width w (HYBRID UPWIND WIDTH) parameters as, $\chi = \frac{1}{2}[1+tanh(\frac{Pe-p}{w})]$ . Tanh is centered ( $\chi=0.5$ ) when Peclet number is at the shifting factor p. Width determines how fast $\chi$ changes with Peclet number as follows:

$\chi=$ 0.5 at Pe=p.
$\chi=$ 0.8808 and 0.1192 at Pe=p+w and p-w.
$\chi=$ 0.9820 and 0.0180 at Pe=p+2w and p-2w.
$\chi=$ 0.9975 and 0.0025 at Pe=p+3w and p-3w.
$\chi=$ 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 $(I - \tau A) G (\Delta P)$ .

“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 ${\bf false}$ .

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 $k$ is: $rate*(Y_{fs,k} - Y_k)$ 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: $rhs+=rate*(Y_{fs,k} - Y_k)$ and $hs+=rate$ . 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 $T = 2320$ , this represents a discontinuous change in absorption coefficient)

Brewster:

0.000094

4

300 0.0821

1000 0.10639

2320 0.002384

10000 0.74352 ( $T = 10000$ 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: $\phi^{n+1} = \phi^{n}$
Forward Euler: $\phi^{n+1} = \phi^{n} + \Delta t \dot \phi$
Adams Bashforth: $\phi^{n+1} = \phi^{n} + {{\Delta t} \over {2} }( 3 \dot \phi^n - \dot \phi^{n-1})$ .

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

   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 $C_{deris} (\rho_F-\rho) g_j k^{0.5}$ where $C_{deris}$ 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 $C_{deris} \Delta k^{0.5} (|\nabla\rho\times g| - \nabla\rho\cdot g)$ where $C_{deris}$ 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, $G_B = \beta {\mu_t \over Pr_t} { \partial T \over \partial x_j } g_j.$ For the turbulent kinetic energy, $G_B$ augments the right hand side while for the dissipation rate equation, $C_{\epsilon1}' C_{\epsilon4} {1 \over T} G_B$ 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 $k$ - $\epsilon$ 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, $G_B = \rho_{ref} {\mu_t \over Pr_t} { \partial (1/ \rho) \over \partial x_j } g_j.$ For the turbulent kinetic energy, $G_B$ augments the right hand side while for the dissipation rate equation, $C_{\epsilon1}' C_{\epsilon4} {1 \over T} G_B$ 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.

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 $T_{visc}/\sigma_i$ . 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 $2*\nu*\mu_t* \left( \frac{\partial^2 u_i}{\partial x_k \partial x_j} \frac{\partial^2 u_i}{\partial x_k \partial x_j} \right)$ .

This source term is calculated using a two pass shape function evaluation. The first pass calculates the standard derivatives, $\partial u_i/ \partial x_j$ . 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 $K_{wall} = u_{\tau}^2/\sqrt{C_{\mu}}$ . 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 $k$ - $\epsilon$ model. The model uses the turbulence model parameters $C_{bvg}$ and $C_{\epsilon3}$ .

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 ( $f$ ) on either the specified volume (blocks) or surface (sidesets) and save the result as a global variable. The function $f$ can depend on time and space ( $t$ , $x$ , $y$ , $z$ ) and any nodal variable.

On volumes this is:

$F = \int_{V} f dV$

while on surfaces it is:

$F = \int_{A} f dA$

Average

Perform a volume or area weighted average of the specified scalar function ( $f$ ) on either the specified volume (blocks) or surface (sidesets) and save the result as a global variable. The function $f$ can depend on time and space ( $t$ , $x$ , $y$ , $z$ ) and any nodal variable.

On volumes this is:

$F = \frac{\int_{V} f dV}{\int_{V} dV}$

while on surfaces it is:

$F = \frac{\int_{A} f dA}{\int_{A} dA}$

Sum

Find the nodal summation of the specified scalar function ( $f$ ) on either the specified volume (blocks) or surface (sidesets) and save the result as a global variable. The function $f$ can depend on time and space ( $t$ , $x$ , $y$ , $z$ ) and any nodal variable.

Min

Find the nodal minimum of the specified scalar function ( $f$ ) on either the specified volume (blocks) or surface (sidesets) and save the result as a global variable. The function $f$ can depend on time and space ( $t$ , $x$ , $y$ , $z$ ) and any nodal variable.

Max

Find the nodal maximum of the specified scalar function ( $f$ ) on either the specified volume (blocks) or surface (sidesets) and save the result as a global variable. The function $f$ can depend on time and space ( $t$ , $x$ , $y$ , $z$ ) and any nodal variable.

L2_Norm

Find the nodal L2-norm of the specified scalar function ( $f$ ) on either the specified volume (blocks) or surface (sidesets) and save the result as a global variable. The function $f$ can depend on time and space ( $t$ , $x$ , $y$ , $z$ ) and any nodal variable.

On volumes this is:

$F = \sqrt{\int_{V} f^2 dV}$

while on surfaces it is:

$F = \sqrt{\int_{A} f^2 dA}$

Global

Evaluate a global function ( $f$ ) and save the result as a global variable. The function $f$ 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 ( $f$ ) on either the specified volume (blocks) or surface (sidesets) and save the result in a nodal field. The function $f$ can depend on time and space ( $t$ , $x$ , $y$ , $z$ ) 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 $f$ 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 ( $t$ , $x$ , $y$ , $z$ ) and any nodal variable.

$F = \int_{A} \vec{f} \cdot \vec{dA}$

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 ( $t$ , $x$ , $y$ , $z$ ) 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	–