Flow Surface dialog box (Flow/ESC/Multiphysics)

Option	Description
Type	Specifies the type of Flow Surface the software creates.Embedded Flow SurfaceModels a surface that contacts the fluid on both sides.Embedded Flow Surface With ObstructionsModels a surface that contacts the fluid on both sides, and has small obstructions on or near the surface (such as PCB components) that cause flow and convection effects.Boundary Flow SurfaceModels a surface that contacts the fluid on one side.Boundary Flow Surface With ObstructionsModels a surface that contacts the fluid on one side and has small obstructions attached to the surface (such as PCB components) that cause flow and convection effects.
Name
Name	Lets you specify 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.
Flow Surface Region and Flow Surface Obstructions
The Flow Surface Region group appears for all types. The Flow Surface Obstructions group appears only for Embedded Flow Surface With Obstructions or Boundary Flow Surface With Obstructions types.
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 define the flow surface region. In the Flow Surface Obstructions group, it lets you specify the faces or elements that define the obstructions.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.
Surface/Top Surface/Bottom Surface
The Surface group appears for Boundary Flow Surface or Boundary Flow Surface With Obstructions types.The Top Surface and Bottom Surface groups appear for Embedded Flow Surface or Embedded Flow Surface With Obstructions types.
Wall Treatment	Specifies how the flow solver models the near-wall region of a flow surface.No Slip WallResolves the flow field in the near-wall region, including the viscous sublayer. Your model requires a finer mesh near the wall.Slip WallEliminates any surface drag calculations for the surface of the blockage and assigns automatic convection properties.Wall FunctionProvides near-wall boundary conditions for the momentum and turbulence transport equations without resolving the viscous sublayer. Applicable only when you also select K-Omega, SST — Shear Stress Transport, or LES — Large Eddy Simulation from the Turbulence Model list on the Solution Details page in the Solution dialog box.Note: The implementations of the Standard K-Epsilon, RNG K-Epsilon, Realizable K-Epsilon and Mixing Length turbulence models always use wall functions.Hybrid Wall FunctionUses enhanced wall functions that are less sensitive to the first layer y+ values and provides a more robust performance upstream of the separation point in comparison with standard wall functions. Hybrid wall functions transition smoothly between wall-resolved (no slip) and wall function corrected treatments based on local grid quality.Applicable only when you also select K-Omega or SST — Shear Stress Transport from the Turbulence Model list on the Solution Details page in the Solution dialog box.Note: A single solution can only contain one type of wall functions: you cannot specify standard wall functions on some surfaces and hybrid wall functions on others. A combination of flow surfaces with and without wall functions is allowed.For more information see Meshing for turbulence modeling.
Wall Friction	Available when Wall Treatment is set to anything except Slip Wall.Specifies how the software computes wall friction. Smooth – With FrictionApplies the drag on a smooth wall. The flow solver computes the drag force by integrating the shear stress over the wall surface.Rough Applies drag on a rough wall. The roughness effect is included in computation using the Sand Grain Roughness Height value that you specify. Surface roughness tends to increase convection heat transfer by introducing flow turbulence.Note: The specified Sand Grain Roughness Height value must not exceed the size of the fluid elements next to the surface.
Convection Properties	Controls how the Flow Blockage convects to the fluid.By default, all Solid type Flow Blockage objects convect to the fluid using convection properties defined in the 3D Flow node in the Solution dialog box. You can override these properties with a Convection Properties type modeling object. Select Automatic to allow the flow solver to calculate local convection properties for each element on the Flow Blockage.Select a Convection Properties type modeling object from the list to apply those convection properties to the blockage, or click Create Modeling Object to define a new modeling object.Click Modify Selected to modify the specified modeling object.
Semi-Permeable Interface
The Semi-Permeable Interface group appears only for the Boundary Flow Surface type.To model semi-permeable surfaces, you must have humidity present in your model.
Semi-Permeable Interface	Indicates that the boundary flow surface diffuses humid air to the external ambient region. The boundary flow surface is semi-permeable in the sense that the velocity is zero at the boundary, thus there is no convection between the enclosure and the external ambient region. Use this option to model semi-permeable membranes such as GORE-TEX® textiles.You set the type of permeable diffusion in the Permeability Type list.Humidity PermeabilityDiffuses humidity to ambient air given a diffusion resistance value. There is no explicit flow or head loss associated with this permeability type. You specify a constant or temperature-varying diffusion resistance value in the Diffusion Resistance box and the ambient humidity using the External Conditions list.Mixture PermeabilityAllows for the exchange of humid air across the semi-permeable surface by equalizing pressures across the interface. The humid air can cross the interface in either direction depending on the pressure difference across the interface. You specify a constant head loss factor in the Loss Coefficient box.The equation for this model uses the ambient pressure that you define on the Ambient Conditions page of the Solution dialog box.
External Conditions	Appears when Permeability Type is set to Humidity Permeability.Specifies the humidity at the boundary.AmbientSpecifies the ambient humidity at the boundary, which you define on the Ambient Conditions page of the Solution dialog box.External Conditions modeling objectSpecifies the humidity 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.Note: The flow solver ignores the values for temperature and turbulence characteristics in the External Conditions modeling object that is referenced by a Boundary Flow Surface simulation object.
Rotation/Translation Parameters
Rotating/Translating Surface in Shear	Moves the flow surface with the flow using the type of movement that you set in the Motion Type list.TranslatingDefines a displacement direction and velocity of the translating surface. Use the Specify Vector options to specify the direction of the surface displacement and the Velocity box to specify the velocity at which the translating surface is moving.RotatingDefines an axis and a constant rate of rotation of the rotating surface. You specify the rate of rotation in the Rotation Rate dialog box.
Rotation Axis	Appears when Motion Type is set to Rotating.Specifies the axis around which the flow surface rotates.Global Cyclic AnalysisAppears if you defined the cyclic symmetry cylindrical coordinate system in the FEM. Rotates the flow surface around the Z-axis of the cyclic symmetry cylindrical coordinate system. User-DefinedLets you specify the axis around which the flow surface rotates. Use the Specify Vector options to specify the direction of revolution, and use the Specify Point options to specify the location of the axis.
Particle Tracking
Appears for Embedded Flow Surface and Boundary Flow Surface types.
Particle Impact Type	Specifies whether the particles stick to the flow surface or rebound.ReboundIndicates that the particles rebound on the walls of the flow surface. The flow solver needs a value for the coefficient of restitution, α, to compute how much energy the particle loses when it hits the wall. You set the value in the Coefficient of Restitution box. The specified value must be: 0 ≤ α ≤ 1.StickIndicates that the particles stick to the walls.
Impact Report	Generates the ParticleAndImpactTrackingSummary.dat file which contains two tables:The Particle Tracking Summary table lists the number of injected and ejected particles in total for your model and per boundary condition.The Particle Surface Impact and Screen Pass-Through Tracking Report table lists the number of particles that impact walls in your model per injection boundary condition and the number of particles that pass through screens per injection boundary condition.The file is generated in the simulation’s run directory.
Fluid-Structure Interactions
Appears for Embedded Flow Surface and Boundary Flow Surface types in the Multiphysics solver environment.
Fluid-Structure Coupling	Specifies the fluid-structure coupling at fluid-structure interfaces.NoneIndicates that there is no exchange of data between the structural and flow solvers.CoupledIndicates that the structural and flow solvers exchange data at each coupling time.

How do I

Create a flow surface

Learn more

Flow Surface

Meshing for flow surfaces

Understanding flow surfaces

Modeling flow surface obstructions

Convection Properties

Modeling convection

Two-way fluid-structure interaction

Look up more details

Meshing for turbulence 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 Surface dialog box (Flow/ESC/Multiphysics), 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 } });