Flow Boundary Condition dialog box – Inlet Flow options

Name
Name	Sets a name for the simulation object.Description opens an editor that lets you type a description for the boundary condition.
Destination Folder
Simulation Object Container	Specifies the folder in the Simulation Navigator in which the boundary condition will be stored. The list includes the root container and existing folders that you created using the New Folder command. Examples of a root container include Load Container, Constraint Container, and Simulation Object Container.
Folder Manager	Displays a hierarchical listing of existing folders. To create a new folder, right-click any level of the hierarchy and choose New Folder.
Inlet Region
Group Reference	Applies the boundary condition to the selected group.For more information, see Group Reference options.
Select Object	Lets you select the faces or elements to specify the boundary of the flow domain.Excluded lets you remove individual entities from within your selected object.
Stacked Smart Selector Methods	Opens the Smart Selector Methods dialog box where you can specify a progression of smart selection filters.For more information, see Smart Selector Methods dialog box.
Magnitude
Mode	Specifies how you define the flow conditions at the fan.VelocitySpecifies the flow velocity at the inlet. The flow velocity is the speed of the fluid movement normal to the boundary condition surface. You define the magnitude with a constant value in the Velocity box. When the flow is deflected using the Alignment Along Vector option or the Swirl option, the volumetric flow rate is preserved.Velocity VectorSpecifies the flow velocity vector components at the inlet. The components can either be constant, or vary with respect to time and spatial variables. You can use a formula field, a table of fields, or a 4D field to define how the flow velocity vector components vary with respect to time and spatial variables.To define constant velocity vector components, set the Velocity list to Expressions. You define the flow velocity vector components in the Vx, Vy, and Vz boxes using an expression. To define the velocity vector components using tabular data, set the Velocity list to Fields. You can define a formula field, a table of fields, or a 4D field. You can also define the Scale Factors for the flow velocity vector components in the Vx, Vy, and Vz boxes.Mass FlowSpecifies the mass flow per unit of time through the inlet. You define the magnitude with a constant value in the Mass Flow box.Volume FlowSpecifies the volume flow per unit of time through the inlet. You define the magnitude with a constant value in the Volume Flow box.Pressure RiseSpecifies the change in pressure across the inlet. You define the magnitude with a constant value in the Pressure Rise box. The pressure that you specify is a total pressure, relative to ambient pressure. Total pressure is the static pressure plus the dynamic pressure.Fan CurveUses a fan curve definition to specify the relationship between flow rate and static pressure rise across the inlet in the Fan Curve box. In Simcenter 3D Electronic Systems Cooling, you can select a pre-defined fan curve from the manufacturing data when you click Fan Catalog . With each of these options, if you use a field definition to define flow conditions and the time is outside of the defined field values, the software uses the last value defined by the field until the specified End Time of the analysis. The end time is specified on the Transient Setup page of the Solution dialog box.For more information, see Additional magnitude options.
External Conditions
External Conditions	Specifies the temperature, humidity, and turbulence characteristics at the boundary.AmbientSpecifies ambient flow conditions at the boundary, which you define on the Ambient Conditions page of the Solution dialog box.External Conditions modeling objectSpecifies the flow conditions at the boundary through the selected External Conditions modeling object.You can also select a previously defined External Conditions modeling object from the list or click Create Modeling Object to define a new modeling object.Click Edit to modify the specified modeling object.
External Absolute Pressure	Appears only when Pressure Rise is selected from the Mode list.Controls how the absolute pressure at the inlet is defined.Select Ambient to specify that the value is equal to the Absolute Pressure Value specified on the Ambient Conditions page of the Solution dialog box.Select Specify to assign the value for the external absolute pressure. You define the value in the Pressure Value box.
Turbulence Characteristics	Specifies which method is used to specify turbulence properties of fluid based on available data derived from experiment or standard references.AutomaticLets the solver compute automatically turbulence characteristics.Turbulence Characteristics modeling objectSpecifies the method for calculation initial turbulence quantities through the selected Turbulence Characteristics modeling object.You can also select a previously defined Turbulence Characteristics modeling object from the list or click Create Modeling Object to define a new modeling object.Click Edit to modify the specified modeling object.For more information, see Turbulence Characteristics.
Head Loss
Head Loss	Appears only when Pressure Rise or Fan Curves is selected from the Mode list.Lets you define a pressure drop across the inlet due to a planar device, such as a screen or filter. Choose a previously defined Planar Head Loss modeling object from the list or click Create Modeling Object to create a new one. See Planar Head Loss.
Heat Generated at Inlet
Heat Load	Lets you specify a positive or a negative heat load transferred from the device to the fluid passing through it into the flow domain.
Tracer Fluid
Available if you choose an External Conditions modeling object from the External Conditions list.
Tracer Fluid	Defines the mixing of one or more tracer fluids entering the fluid domain through the inlet.None specifies that no mixing occurs.Specify Fractions lets you specify a previously defined Tracer Fluid modeling object and a matching mass fraction. See Tracer Fluid for more information.
Tracer Fluid List	Opens the Modeling Objects Manager where you can select or create a Tracer Fluid modeling object.See Model a tracer fluid for more information.
Tracer Fluid Mass Fractions	Sets the mass fractions for the Tracer Fluid modeling objects you select in the Tracer Fluid List.As a good practice, enter values from 0 to 1 for each mass fraction. The percentage of air is calculated as 1–∑Mass Fractions.If the sum of the mass fractions you enter is greater than 1, the values are normalized.You can use Cut , Copy , and Paste commands.
Mixture
Available if you choose an External Conditions modeling object from the External Conditions list.
Mixture	Specifies the mass fractions for the components of a mixture for the ambient fluid domain.NoneIndicates that there is no mixture entering the fluid domain.Homogeneous Gas MixtureSets the mass fractions for the homogenous mixture components.Immiscible Fluid MixtureSets the area fraction of the tracked fluid in the immiscible mixture entering the fluid enclosure. The area fraction value must be between 0 and 1, and it can vary with time in a transient analysis. If it is not defined, the flow solver assigns a value of 1. You define the value in the Tracked Fluid Area Fraction box.
Mixture Mass Fractions	Appears when Mixture is set to Homogeneous Gas MixtureSets the mass fractions for the homogenous mixture components.As a good practice, enter values from 0 to 1 for each mass fraction. If the sum of the mass fractions you enter is greater than 1, the values are normalized.You can use Cut , Copy , and Paste commands.
Flow Direction
Alignment	Specifies the general direction of the fluid flow.Normal to Face specifies that the fluid enters normal to the inlet. This is the appropriate alignment for most cases.Along Vector lets you specify a vector along which the fluid enters. This allows you to model the effect of devices that deflect the fluid flow, such as louvers on a fan or vent. Use the Specify Vector options to specify the direction of the flow.
Swirl	Appears when Alignment is set to Normal to Face.Models the effect of fan swirl. See Modeling fan swirl for more information.None specifies that there is no fan swirl effect.Fixed Angle specifies that the fluid rotates at the specified angle. You specify the fixed angle value in the Normal to Resultant Velocity Angle box. It is the angle between the device normal and the resultant fluid velocity vector.Radially Varying specifies that the fluid rotates at a varying angle. You specify the value for the rotational velocity of the device in the Rotational Velocity box.
Rotation Axis	Appears when Swirl is not set to None.Specifies the axis around which the fluid swirls when entering the flow domain.Global Cyclic AnalysisAppears if you defined the cyclic symmetry cylindrical coordinate system in the FEM. Swirls the fluid around the Z-axis of the cyclic symmetry cylindrical coordinate system. User-DefinedLets you specify the axis around which the fluid swirls. Use the Specify Vector options to specify the direction of revolution, and use the Specify Point options to specify the location of the axis.
Fan Control
Controller Type	Specifies how the speed of the Flow Boundary Condition is controlled.None specifies that the speed at the boundary condition is not controlled.Thermostat lets you control the speed with a Thermostat modeling object. Choose a previously defined Thermostat modeling object from the list or click Create Modeling Object to create a new one. See Thermostat for more information.Speed Control lets you control the speed based on the temperature of a sensor. Choose a previously defined Fan Speed Controller modeling object from the list or click Create Modeling Object to create a new one. See Fan Speed Controller for more information.
Nominal Fan Speed	If you chose Velocity, Mass Flow, or Volume Flow from the Mode list, the Nominal Fan Speed value corresponds to the specified velocity or flow value (Qnominal). The software obtains the flow rate at a new temperature during the solve using this equation:Qnew = Qnominal × RPMnew / RPMnominalIf you chose Pressure Rise from the Mode list, the Nominal Fan Speed value corresponds to the specified pressure rise value (dPnominal). The software obtains the flow rate at a new temperature during the solve using this equation: dPnew = dPnominal × (RPMnew / RPMnominal)2 If you chose Fan Curve from the Mode list, the software uses the two equations above to compute the fan operating point.

How do I

Create a Flow Boundary Condition

Learn more

Flow Boundary Condition

Flow Boundary Condition types

Working with fan curves

Modeling heat loss or gain in a recirculation loop

Modeling fan swirl

Flow boundary condition modeling

External Conditions

Planar Head Loss

Look up more details

Flow Boundary Condition dialog box– Outlet Flow options

Flow Boundary Condition dialog box – Opening options

Flow Boundary Condition dialog box– Internal Fan options

Flow Boundary Condition dialog box – Recirculation Loop options

Flow Boundary Condition dialog box– Convective Outflow options

Flow Boundary Condition dialog box– Static Pressure options

Flow Boundary Condition dialog box– Bursting Membrane options

Flow Boundary Condition dialog box– Flap options

Defining the mesh size for fluid modeling

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Thermal/Flow, Electronic Systems Cooling, and Space Systems Thermal

Simcenter 3D Thermal/Flow, Electronic Systems Cooling, and Space Systems Thermal boundary conditions

Flow Boundary Condition dialog box – Inlet Flow options, Simcenter 3D 2021.1 Series

© 2020 Siemens

window.mainLanguage="en_US"

window.delivId=""

window.projectId=""

MathJax.Hub.Config({ TeX: { extensions: ["autoload-all.js"] }, tex2jax: { displayMath: [ ] }, "SVG": { scale: 125 } });