Node95 - CFD SUPPORT

Previous: Boundary types Up: Boundary conditions in OpenFOAM Next: Inlet Boundary Conditions

This is an automatically generated documentation by LaTeX2HTML utility. In case of any issue, please, contact us at info@cfdsupport.com.

Boundary conditions

Boundary conditions are set in solution directories (0/U, …)
The most typical case is the velocity is prescribed at the inlet and static pressure is prescribed at the outlet.

Figure: Test case geometry

Boundary conditions in OpenFOAM are divided into two groups by – basic and derived.
Basic boundary conditions by OpenFOAM implementation:

Boundary condition	Description	Variables
fixedValue	constant value at boundary	value
fixedGradient	constant gradient	gradient
zeroGradient	zero gradient (extrapolation)	–
calculated	depending on other quantities	–
mixed	mix from other boundary conditions	refValue, refGradient,
		valueFraction, value
directionMixed	anisotropic BC mixed,	refValue, refGradient,
	valueFraction is tensor	valueFraction, value

OpenFOAM has many derived boundary conditions
Some examples follow
Derived boundary conditions are stored on the path:
- $FOAM_SRC/finiteVolume/fields/fvPatchFields/derived
- or can be found by following command:
  # find $FOAM_SRC -name "*derivedFvPatch*"
  # find $FOAM_SOLVERS -name "*derivedFvPatch*"

Derived boundary conditions based on fixedValue

name	Description	Variables
totalPressure	total pressure is constant,
	static pressure is computed
pressureInletVelocity	if known pressure at inlet	value
	velocity is computed from flux
pressureDirectedInletVelocity	if known pressure at inlet	value,
	velocity is computed from flux	inletDirection
	velocity direction is respected
movingWallVelocity	moving wall	value
surfaceNormalFixedValue	velocity magnitude is kept,	value
	direction is perpendicular
	to domain
turbulentInlet	calculates a fluctuating	referenceField
	variable based on a scale of	fluctuationScale
	a mean value

Derived boundary conditions based on fixedGradient/zeroGradient boundary condition

Name	Description	Variables
fluxCorrectedVelocity	Normal component is computed	value
wallBuoyantPressure	Sets pressure gradient value	value
	according to atmospheric pressure

Derived boundary conditions based on mixed boundary condition

Name	Description	Variables
inletOutlet	switching between fixedValue	inletValue,
	and zeroGradient	value
	depending on flow direction
outletInlet	switching between fixedValue	outletValue,
	and zeroGradient	value
	depending on flow direction
pressureInletOutletVelocity	combination of pressureInletVelocity	value
	and inletOutlet
pressureDirectedInletOutletVelocity	combination of	value,
	pressureDirectedInletVelocity
	and inletOutlet
pressureTransmissive	transmitting supersonic pressure waves	pInf
supersonicFreeStream	transmits shocks to surroundings	pInf, TInf, UInf

Another derived boundary conditions

Name	Description	Variables
slip	slipping wall	–
partialSlip	combines slip and zeroGradient	valueFraction
	depending on valueFraction
	(0 = slip)
noSlip	fixes the velocity to zero	–
	at the walls

Previous: Boundary types Up: Boundary conditions in OpenFOAM Next: Inlet Boundary Conditions

OpenFOAM Training by CFD Support, CFD SUPPORT, info@cfdsupport.com +420 212 243 883 © CFD support, s.r.o., Sokolovská 270/201, 190 00 Praha 9, Czech Republic

Next: Model setting without an Up: Alternative formulation Previous: Alternative formulation Contents Index

Mass Flow Rate - patchMassFlow Function

Function patchMassFlow is included in file controlDict. Definition of forces functions are created in file flux.fun. This function is part of libsimpleFunctionObjects.so library and can evaluate mass flow rate through selected patches:

 massFlowInlet
{
    type                    patchMassFlow;
    region                  spiral;
    functionObjectsLibs     ( "libsimpleFunctionObjects.so" );
    verbose                 true;
    patches
    (
        inflow_inlet
    );
    factor                  1.;
}
massFlowMXP1_spiral
{
    type                    patchMassFlow;
    region                  spiral;
    functionObjectsLibs     ( "libsimpleFunctionObjects.so" );
    verbose                 true;
    patches
    (
        spiral_rotor_mxp_0 spiral_rotor_mxp_1 spiral_rotor_mxp_2 spiral_rotor_mxp_3
        spiral_rotor_mxp_4 spiral_rotor_mxp_5 spiral_rotor_mxp_6 spiral_rotor_mxp_7
    );
    factor                  1.;
}
massFlowMXP1_rotor
{
    type                    patchMassFlow;
    region                  rotor;
    functionObjectsLibs     ( "libsimpleFunctionObjects.so" );
    verbose                 true;
    patches
    (
        rotor_spiral_mxp_0 rotor_spiral_mxp_1 rotor_spiral_mxp_2 rotor_spiral_mxp_3
        rotor_spiral_mxp_4 rotor_spiral_mxp_5 rotor_spiral_mxp_6 rotor_spiral_mxp_7
    );
    factor                  1.;
}
massFlowMXP2_rotor
{
    type                    patchMassFlow;
    region                  rotor;
    functionObjectsLibs     ( "libsimpleFunctionObjects.so" );
    verbose                 true;
    patches
    (
        rotor_drafttube_mxp_0 rotor_drafttube_mxp_1 rotor_drafttube_mxp_2 rotor_drafttube_mxp_3
        rotor_drafttube_mxp_4 rotor_drafttube_mxp_5 rotor_drafttube_mxp_6 rotor_drafttube_mxp_7
    );
    factor                  1.;
}
massFlowMXP2_drafttube
{
    type                    patchMassFlow;
    region                  drafttube;
    functionObjectsLibs     ( "libsimpleFunctionObjects.so" );
    verbose                 true;
    patches
    (
        drafttube_rotor_mxp_0 drafttube_rotor_mxp_1 drafttube_rotor_mxp_2 drafttube_rotor_mxp_3
        drafttube_rotor_mxp_4 drafttube_rotor_mxp_5 drafttube_rotor_mxp_6 drafttube_rotor_mxp_7
    );
    factor                  1.;
}
massFlowOutlet
{
    type                    patchMassFlow;
    region                  drafttube;
    functionObjectsLibs     ( "libsimpleFunctionObjects.so" );
    verbose                 true;
    patches
    (
        outflow_outlet
    );
    factor                  1.;
}

During the computation the results are written down in directory
patchMassFlows_massFlowInlet/0/massFlow,
patchMassFlows_massFlowMXP1_spiral/0/massFlow, …

OpenFOAM Training by CFD Support, CFD SUPPORT, info@cfdsupport.com +420 212 243 883 © CFD support, s.r.o., Sokolovská 270/201, 190 00 Praha 9, Czech Republic

Previous: SIMPLE Algorithm Up: TCFD Solvers Next: Temporal Integration Numerical Scheme
_{This is an automatically generated documentation by LaTeX2HTML utility. In case of any issue, please, contact us at info@cfdsupport.com.}

Spatial Integration Numerical Scheme

Space discretization scheme is limitedLinear, which is central scheme of second order accuracy. There are 55 default OpenFOAM schemes to select:

CoBlended
Gamma
Gamma01
LUST
MUSCL
MUSCL01
Minmod
OSPRE
QUICK
SFCD
SuperBee
UMIST
biLinearFit
blended
clippedLinear
cubic
cubicUpwindFit
downwind
filteredLinear
filteredLinear2
filteredLinear3
fixedBlended
harmonic
limitWith
limitedCubic
limitedCubic01
limitedGamma
limitedLimitedCubic
limitedLimitedLinear
limitedLinear
limitedLinear01
limitedMUSCL
limitedVanLeer
limiterBlended
linear
linearFit
linearPureUpwindFit
linearUpwind
localBlended
localMax
localMin
midPoint
outletStabilised
pointLinear
quadraticFit
quadraticLinearFit
quadraticLinearUpwindFit
quadraticUpwindFit
reverseLinear
skewCorrected
upwind
vanAlbada
vanLeer
vanLeer01
weighted

For more details see e.g. [9], [1] or [3].

Previous: SIMPLE Algorithm Up: TCFD Solvers Next: Temporal Integration Numerical Scheme

OpenFOAM Training by CFD Support, CFD SUPPORT, info@cfdsupport.com +420 212 243 883 © CFD support, s.r.o., Sokolovská 270/201, 190 00 Praha 9, Czech Republic

Boundary conditions ​

Mass Flow Rate - patchMassFlow Function

Spatial Integration Numerical Scheme

Boundary conditions