Solution dialog box — 3D Flow

Option	Analysis/Solution Type	Description
User Defined API File
User Defined API File	Advanced Flow Electronic Systems Cooling****Advanced Thermal-Flow with ESC	Allows you to specify a user-defined API file that is a dynamically linked library (DLL) containing your plugin, which lets you expand the capabilities of the parallel flow solver. You specify the DLL in the Select File box. For more information, see Specify a flow user defined API file and Flow Solver API Manual .
Flow Surface Parameters
Non-fluid 2D and 3D Elements Block Flow	Flow****Coupled Thermal-Flow	Controls if the software calculates friction and convection on polygon faces and bodies meshed with elements having non-fluid properties in contact with the fluid.If you select this option, the flow solver detects all polygon faces and bodies meshed with elements having non-fluid material properties. Where these polygon faces and bodies contact the fluid mesh, the solver models friction and convection using the options specified in the Flow Surface Parameters group. With this option if non-fluid 2D or 3D elements are embedded in the fluid mesh, they block the flow.If you clear this option, the flow solver does not calculate friction and convection on polygon faces and bodies meshed with elements having non-fluid properties in contact with the fluid unless you create a Flow Surface on them, or unless they are part of a Solid type Flow Blockage. With this option if non-fluid 2D or 3D elements are embedded in the fluid mesh, they do not block the flow.
Wall Treatment	Flow****Coupled Thermal-Flow	Appears only when the Non-fluid 2D and 3D Elements Block Flow check box is selected. 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.
Default Wall Friction	Flow****Coupled Thermal-Flow	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.
Default Convection Properties	Flow****Coupled Thermal-Flow	Specifies the default convection properties the solver uses for surfaces in contact with the fluid mesh.Select Automatic to have the solver calculate default convection properties.Select a Convection Properties modeling object to define the convection properties. You can select a previously defined one from the list or select to create a new one.
Reference Temperature for Bulk Heat Transfer Coefficient	Flow****Coupled Thermal-Flow	Defines the temperature the solver uses to calculate the bulk heat transfer coefficient. Ambient uses the Fluid Temperature specified on the Ambient Conditions page. If the ambient Fluid Temperature is defined as time varying, then the software uses the interpolated value at the time step. Local applies the nearest calculated node temperature for each convecting element. Specify applies the temperature you enter in the Reference Temperature box.
Default Particle Impact Type	Flow****Coupled Thermal-Flow	Specifies whether the particles stick to the wall or rebound. This setting applies to all flow surfaces unless you modify it for a specific surface using the Flow Surface simulation object.ReboundIndicates that the particles rebound on the walls of the fluid domain. 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 Default Coefficient of Restitution box. The specified value must be: 0 ≤ α ≤ 1.StickIndicates that the particles stick to the walls.
Characteristic Scales
Length Scales	Flow****Coupled Thermal-Flow	Only required if you selected Fixed Turbulent Viscosity or Mixing Length viscosity model on theSolution Details page of the Solution dialog box.Automatic lets the solver calculate the characteristic scales based on local conditions.Specify lets you define values for Characteristic Length Scale and Fixed Viscosity Mean Flow Velocity Scale.
Additional Parameters
Connect Disjoint Fluid Meshes	Flow****Coupled Thermal-Flow	Allows fluid flow between polygon bodies that have one or more pairs of coplanar faces, even if the nodes of the two fluid meshes are not coincident. Some degradation of performance and accuracy can result.If you do not want that the fluid flow to cross disjoint fluid meshes, clear this check box.Note: This check box only applies for the serial flow solver. The parallel flow solver ignores the state of the check box. When using the parallel flow solver, define the Disjoint Fluid Mesh Pairing simulation object to connect disjoint meshes.
High Speed Flow	Advanced FlowAdvanced Thermal-FlowAdvanced Thermal-Flow with ESC	Activates solver equations to include high speed flow terms. The solver uses the total energy equation to handle subsonic, transonic and supersonic flow regimes. The solver does not support hypersonic flow regime. Depending on the flow speed and the effects you want to model, you may need to set a very small time step on the 3D Flow Solver page in the Solver Parameters dialog box.If you do not want to model high speed flow, clear this check box.Note: High speed flows are not supported by the fractional step parallel flow solver scheme.
Non-Newtonian Fluid	Advanced FlowAdvanced Thermal-FlowAdvanced Thermal-Flow with ESC	Specifies that a defined fluid material has the non-Newtonian properties you specify in a Non-Newtonian Fluid modeling object. You can include as many non-Newtonian fluids in the simulation as you want. You must override the 3D solid mesh collector material definition to apply the properties to the mesh.
Fluid Domain Parameters
Source of Domain Geometry	Flow****Coupled Thermal-Flow	Controls the source of the geometry and obstructions used to create the mesh generated when you use the Fluid Domain simulation object.Idealized or Master Part specifies that the boundary of the fluid mesh is defined by parasolid geometry (visible in part files). Polygon Geometry specifies that the boundary of the fluid mesh is defined by polygon geometry (visible in FEM and Simulation files).Note: Use this option when working with assembly FEMs.
Remove Small Features	Appears when Source of Domain Geometry is set to Idealized or Master Part.Removes small features from the parasolid geometry when meshing using the Fluid Domain simulation object.
Tolerance	Available when Remove Small Features is selected.Controls the level of simplification of the parasolid geometry.Relative allows you to specify a Value that represents the minimum size, relative to the size of the fluid volume, below which features are ignored for mesh creation.Absolute allows you to specify an absolute Value that represents the minimum size below which features are ignored for mesh creation.
Other Geometry Features	Appears when you set Source of Domain Geometry to Polygon Geometry.Controls what kind of internal obstructions the software detects and meshes around when building the mesh.From Polygon Geometry instructs the software to detect any polygon geometry within the fluid domain.From Mesh instructs the software to detect any FEM meshes within the fluid domain.Ignored instructs the software to not detect objects within the fluid domain.
Fluid Domain Mesh Parameters
Allow mesh size variations inside fluid domains	Flow****Coupled Thermal-Flow	Enables variations in element size in the fluid domain. The software increases the element size towards the center of the volume.
2D Element Shape Threshold	Specifies how the element shape quality of the surface seed mesh is determined. You can modify the element’s reverse aspect ratio, skewness, or maximum angle.Use Mesh DefaultUses the default reverse aspect ratio value of 1/6.Aspect RatioSets the desired value for the reverse aspect ratio of the triangular elements. The aspect ratio, AR, is defined as:AR = L/Swhere L is the longest edge of the element (1) and S is the shortest altitude (2).The reverse aspect ratio value ranges from 0 to 1.SkewSets the desired value for the skewness of the elements. The skewness is defined as:Skewness = (Aoptimal —Aelem)/Aoptimal where Aoptimal is the optimal area of the 2D element and Aelem is the actual area of the element.The skewness value ranges from 0 to 1.Maximum AngleSets the desired value for the maximum angle of the triangular elements. The maximum angle ranges from 145 degrees to 180 degrees.
3D Element Shape Threshold	Specifies how the shape quality of the fluid volume elements is determined. You can modify the element’s reverse aspect ratio, skewness, or maximum angle.Use Mesh DefaultUses the default reverse aspect ratio value of 1/12.Aspect RatioSets the desired value for the reverse aspect ratio of the tetrahedral elements. The aspect ratio, AR, is defined as:AR = L/Swhere L is the longest edge of the element and S is the shortest altitude.The reverse aspect ratio value ranges from 0 to 1.SkewSets the desired value for the skewness of the elements. The skewness is defined as:Skewness = (Voptimal —Velem)/Voptimal where Voptimal is the optimal volume of the element and Velem is the actual volume of the element.The skewness value ranges from 0 to 1.Maximum AngleSets the desired dihedral angle of the tetrahedral elements. The maximum angle ranges from 145 degrees to 180 degrees.
Element Shape Threshold Refinement	Refines the mesh in order to satisfy the specified shape metrics. You must specify a refinement factor, ranging from 0 to 1, using the 2D/3D Element Shape Threshold Refinement Factor slider.The mesh, MSnew, is refined using the following equation:MSnew = RF x MSwhere RF is the refinement factor and MS is the initial mesh size.
Element Growth Through Volume	Enables the rate of transition of the mesh size from finer to coarser regions. You specify the rate of transition of the mesh size, ranging from 0 to 1, using the Element Growth Rate Through Volume slider.For an element growth through volume value of 1, the mesh will double in size with each element. As this value decreases, the transition in element size will occur for fewer elements. For a value of 0, the mesh will jump from a fine to coarse mesh with no transition.
Surface Curvature Based Variation	Enables the control of the level of geometric approximation of the surface when generating the mesh. You must specify the curvature refinement, ranging from 0.01 to 0.4 using the Surface Curvature Based Size Variation slider.The software sets the mesh size using the distance, d (3), between the edge (1) and the curve (2), and the length, h (4), of the element edge. The mesh size is selected such that d/h is less than the specified surface curvature value.

How do I

Create disjoint fluid mesh pairings

Learn more

Solution options

Fluid Domain

Non-Newtonian Fluid

Convection Properties

Setting turbulence scale values

Joining fluid meshes

Look up more details

Solution dialog box —Solution Details

Solution dialog box — Solution Units

Solution dialog box — Ambient Conditions

Solution dialog box — Initial Conditions

Solution dialog box —Restart

Solution dialog box —Thermal

Solution dialog box —Transient Setup

Solution dialog box — Results Options

Solution dialog box (Mapping) — Mapping Details

Solution dialog box (Mapping) — Optional Output

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

Solution dialog box — 3D Flow , 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 } });