Specific Derived Parts Reference

Implicit Section Properties

Section Mode

Defines whether the part includes a single or multiple sections.

Option	Activated Child Nodes
Single Section Specifies a single section (default), meaning that there is only one instance of the section within the derived part.	Single section Provides an Offset value for the implicit section, which allows you to offset the section from its original location. For planes, this value is the offset distance along the normal from the origin, and for cylinders or spheres, it the offset value for the radius.
Multiple Sections (range) Specifies a range of sections that are evenly distributed between the start and end offset section positions.	Multiple Sections (range) Provides the total Number of Sections to create, and the Offset Range, which is the offset position of the first and last sections. For planes, the offset position is the distance along the normal from the origin, and for cylinders or spheres, it is the offset value for the radius.
Multiple Sections (delta) Specifies a pattern of sections. This pattern uses the total number of sections and the incremental distance between each section.	Multiple Sections (delta) Provides the total Number of Sections to create, the Starting Offset, that is the distance of the first section along the axis normal to the section, or the first offset radius for spheres or cylinders, and the Delta Value, that specifies the incremental offset between successive sections.
Multiple Sections (arbitrary) Allows you to specify a series of sections that are based on individual offset values.	Multiple Sections (arbitrary) Specifies a series of sections using offset values that you enter in a comma-separated list. For example, setting Offsets to [0.0, 0.01, 0.05, 0.09, 0.1] creates 5 offset sections at the specified offset distances. For planes, the offset value is the distance along the normal from the origin, and for cylinders or spheres, it is the offset value for the radius.

Input Mode

Line Section: specifies two coordinates with one of two modes.

Option	Activated Child Nodes
Point to point Uses two specified points.	Point to point Specifies the Start point and End point of the line.
Point with offset Uses a point and a direction.	Point with offset Specifies the origin (Point) and non-normalized direction (Offset).

Note	Consider the following as you choose your property settings:

• Vector field functions ($${fieldFunction}) are acceptable for property table entries but not for entries into the in-place dialog that appears with an open scene.
• Settings between input modes are not connected, that is, changing the Start point for the Point to point node does not change the Point setting of the Point with offset node.
• All four variables can be added to a Screenplay timeline; however, only those corresponding to the active Input Mode vary. For example, if Point to point is selected, Point and Offset have no effect on the Screenplay animation.

Displayed Index

Controls the display of sections when a multiple mode is used. Enter either a positive integer to display the corresponding section, or a value of -1 to display all sections.

Infinite Line

Line Section: when activated, projects an infinite line that cuts through the entire domain. Otherwise the line is a segment defined by the origin-direction or point-to-point input.

Origin

Plane Section/Constrained Plane Section: a Cartesian position vector that defines the origin of the plane. You can include units.

Cylinder Section: a Cartesian position vector that defines the origin of the cylinder axis. You can include units.

Sphere Section: a Cartesian position vector that defines the location of the center of the sphere. You can include units.

Normal

Plane Section/Constrained Plane Section: a Cartesian position vector that defines the second point through which the plane normal passes. The first point is the origin of the selected Coordinate System. You can include units.

Orientation

Cylinder Section: a Cartesian position vector that defines the second point through which the cylinder axis passes. The first point is the origin of the selected Coordinate System. You can include units.

Radius

Cylinder Section/Sphere Section: the radius of the cylinder or sphere section. You can include units.

Surface Input Option

Arbitrary Section: Specifies the source of the input geometry. The available options are File, that allows you to import arbitrary STL data, and Part Surfaces, that allows you to select one or more of the existing CAD part surfaces in the simulation.

Extract Approximate Faces

Arbitrary Section: when deactivated, the arbitrary section retains its original surface geometry and slices through the sample region. When activated, Simcenter STAR-CCM+ creates an approximation of the surface that maps to the closest mesh cell faces. This option is faster because it does not have to compute the intersection between the section’s surface geometry and the part or region.

Flip Orientation

Arbitrary Section: when activated, Simcenter STAR-CCM+ reverses the directions of the normal vectors of the sample surface faces. The results become evident in reporting for relevant quantities such as mass flux. When deactivated, the face normals are right-hand oriented with respect to the counter-clockwise winding order of the original triangles in the section geometry.

Implicit Section Right-Click Actions

Re-Import Data...

Constrained Plane: Imports data from either an STL or VTK file. This option can be used to replace data that are imported during the creation of this derived part.

Export Loop...

Constrained Plane or Arbitrary: Exports the polygon bounding the constrained plane section to an external an STL file.

Isosurface Properties

Scalar Field

Specifies the scalar field function upon which the isosurface is based. See Field Functions.

Mode

Specifies whether a single isosurface or multiple isosurfaces are created.

Option	Activated Child Nodes
Single Allows you to create one isosurface corresponding to a single scalar value.	Value Within the properties of this node, you can set the Isovalue, that specifies the scalar value for the isosurface.
Multiple (range) Allows you to create multiple isosurfaces corresponding to a range of equally spaced scalar values.	Values (range) Within the properties of this node, you can specify the Number of isosurfaces, that is the total number of equally spaced isosurfaces in the range, and the Isovalue Range, which is the lowest and highest values in the range of isosurfaces.
Multiple (arbitrary) Allows you to create multiple isosurfaces corresponding to a set of scalar values that you specify with numeric entries.	Values (arbitrary) Within the properties of this node, you can specify the Isovalues, that is, a list of scalar values for the multiple isosurfaces. When you set this property by clicking (Custom Editor), the Values (arbitrary) - Isovalues dialog appears. In the dialog, you can click Query to select a scalar range automatically. You can also click Auto Generate Values to select the isovalues automatically.
Closed	When activated, Simcenter STAR-CCM+ creates a closed or nearly-closed surface bounded by the isosurfaces from the regions or geometry parts, and the boundaries or part surfaces, such that the field in the closed space has values less than the specified isovalue. This option is useful in topology optimization studies when you want to extract a solution-generated surface and use it in further simulations. The derived part can be meshed and evaluated with the flow solver. See Validate the Optimized Design.

Threshold Properties

Scalar Field

Specifies the field function that is used to determine the threshold range. See Field Functions.

Range

Specifies the minimum and maximum of the threshold range.

Mode

Specifies how to set the threshold with respect to the specified scalar range:

• Between: the threshold encompasses cells with all values between the minimum and the maximum of the Range.
• Above Max: the threshold encompasses cells with values greater than the maximum of the Range.
• Below Min: the threshold encompasses cells with values less than the minimum of the Range.
• Outside: the threshold encompasses cells with values less than the minimum and greater than the maximum of the Range.

Scalar Warp Properties

Scalar Field

Specifies the scalar field function upon which the warp surface is based. See Field Functions.

Scale Factor

Specifies the scale factor for the warp surface.

Vector Warp Properties

Vector Field

Specifies the vector field function upon which the warp surface is based. See Field Functions.

Relative or Absolute Coordinates

Lets you control the "base" vector, the original position or the updated position:

• Relative: refers to the updated position.
• Absolute: refers to the original position.

Scale Factor

Specifies the scale factor for the warp surface.

In finite element (FE) solid stress applications, use this feature for very small deformations that need to be exaggerated for visualization. For example, if the maximum magnitude of the displacement vector is less than 5% of the maximum model dimension, scale the warp to 20%.

Auto-scaling

When activated, automatically calculates the scale factor based on the sizes of the vector warp and its input parts.

This option is especially useful with visualization of very small and very large warps. When a vector warp is too small to see, Simcenter STAR-CCM+ calculates an increased scale factor to make the deformation visible. Also, for very large warps, a smaller scale factor is calculated.

Auto-scale Value

When Auto-scaling is activated, displays the automatically calculated value of the scale factor. Otherwise the displayed value is 0.0.

Streamline and Constrained Streamline Properties

Vector Field

Selects the type of vector field function to show, such as velocity or flow direction. See Field Functions.

Seed Type

Specifies how the seed point is clustered and defined:

Option	Activated Child Nodes
Point Uses a single point or a cloud of points as the seed. Use this option only when you have a particular set of points, which you could obtain by cutting a surface with a plane or drawing an isosurface.	Point Seed Allows you to define the point seed by setting the following properties: Center: allows you to specify the position of the point cloud. Radius: specifies the radius of the point cloud. It should remain at the default value of zero if you use only one point. The units can be changed by typing them in after the values. Resolution: specifies the number of points in the point cloud.
Line Uses a line of points as the seed. As with the point seed, you should have a specific set of points to use this option. Moreover, the line seed would be effective only on a perfectly flat surface.	Line Seed Allows you to define the line seed by setting the following properties: Line Point 1: allows you to specify the position of one end point of the line. Line Point 2: allows you to specify the position of the other end point of the line. Resolution: specifies the number of evenly spaced points along the line.
Part Uses an existing surface, line, or point part as the seed. Regions cannot be selected. The part (source) seed takes its points from one or more existing parts, therefore it is certain to create a streamline or constrained streamline that lies directly on the part surfaces. This type of seed is the recommended option. When using a part seed, you can use the in-place dialog to specify the Part U-Resolution and Part V-Resolution. These properties allow you to specify the maximum number of points extracted from the part in the u- and v- directions. See Defining a Streamline. Note For a part seed, the chosen part must exist within the same representation as the region containing the solution through which Simcenter STAR-CCM+ integrates the streamline. As such, you cannot use geometry part surfaces for the seed part, as the geometry representation has no solution data.	Source Seed Allows you to define the seed part by setting the following properties: Seed Parts: allows you to select the parts to be used as the seed. Regions are not included among the options. On Ratio: the ratio of available vertices to the maximum numbers of seed points specified for the u- and v-directions. This value is automatically calculated by Simcenter STAR-CCM+. It is recalculated each time you change the u or v points or the Seed Parts property. Randomize: when activated, a random pattern of points is used for the seed points. When deactivated, the vertices of the parts are used for the seed points. It is useful to randomize if the Part uses a highly unstructured grid or mixture of fine and coarse grids. N Grid Points: specifies the maximum numbers of seed points to use in the u- and v- directions. If the number of vertices on the part is less than either value, the number of vertices is used.

Integration Solver

Allows you to select the Runge-Kutta integration solver. The available options are 2nd-Order RK, 4th-Order RK, and Adaptive-Step RK, which activate corresponding child nodes: 2nd Order Integrator, 4th Order Integrator, and Adaptive Integrator. You can define the integration process by setting the properties of the integrator child nodes:

• Integration Direction: specifies the direction of integration from the seed location. The available options are:
  • Forward: the integration proceeds in the forward direction (for instance with the flow if velocity is the vector field).
  • Backward: the integration proceeds in the backward direction (for instance against the flow if velocity is the vector field).
  • Both: the integration proceeds both forward and backward from the seed location.
• Initial Integration Step: specifies the initial integration step size in units of cell length. Reducing the value creates a higher resolution for the streamlines.
• Maximum Error: the maximum allowable error in integration before step size is adjusted.
• Maximum Integration Step: specifies the maximum integration step size in units of cell length.
• Maximum Propagation: specifies the maximum length of the streamlines in units of cell length.
• Max Steps: specifies the maximum number of integration steps.

Rotation Scale

The scale factor for twist.

Wall Treatment

When activated, Simcenter STAR-CCM+ forces the streamlines to be wall-parallel at boundaries. This option is activated by default.

(m', theta) Warp Properties

Rotation Origin

Sets the rotation origin for an (m', theta) warp.

Rotation Axis

Sets the rotation axis for an (m', theta) warp.

Tangential Axis

Sets the tangential axis for an (m’, theta) warp.

Separation/Attachment Line Properties

Display Attachment Lines

Toggles whether lines displaying flow attachment are displayed or not.

Display Separation Lines

Toggles whether lines displaying flow separation are displayed or not.

Vector Field

Specifies the vector field that is used by the algorithm to extract the separation/attachment line. This must be set to wall shear stress or cell relative velocity. If you use a different three-dimensional vector field, it does not produce valid results.

Line Quality

Filters lines where the angle between the extracted separation/attachment line and the flow vector are below the user-defined value. The quality is entered on a scale of 0.0 to 90.0 degrees.

Line Strength

Sets the strength of the separation/attachment. This setting is used to filter out weak results. Line strength is not a physical quantity, but a filtering property. The strength is entered on a scale of 0–1, where 0 includes all separation/attachments, and 1 includes only the strongest results.

Minimum Line Length

Sets the minimum separation/attachment line length. Separation/attachment lines which are shorter than this value are eliminated.

Vortex Core Properties

Vortex Quality

Computes the angle between the extracted core line and the velocity vector at this position. Small angles mean high quality; this may not apply to all simulation data.

Vortex Strength

Sets the strength of the rotational motion. This setting is used to filter out weak vortices.

Minimum Core Length

Sets the minimum length of a line to be used by a vortex core. Below this setting, the core lines are eliminated.

Vector Field

Specifies the vector field that is used by the algorithm to extract the vortex core. This must be set to velocity. If you use a different three-dimensional vector field, this would not lead to a valid result.

Average Surface Properties

Parameterization

Selects an axisymmetric parameterization that includes the input parts chosen for this derived part. Any axisymmetric parameterization that does not include all the input parts chosen for the derived part does not appear in the drop-down list.

Weighting

Determines whether and how to apply weighting as follows:

• None—no additional functions are multiplied by the cell field function value; regardless of weight function, the line segment through the cell is used.

  The closest equivalent is a Riemann sum, where each cell contributes the cell value multiplied by the length of the bin-center line segment. The bin-center line segment has a constant span-wise and flow-wise coordinate located at the geometric center of the bin and runs in the circumferential direction.

• Scalar Function—multiplies the cell scalar of your choice by the cell field function value when computing the average.
• Mass—multiplies the cell field function value by cell mass when computing the average. For this option to be available, the field function Density must be present in the simulation.
• Mass Flow—multiplies the cell field function value by the mass flow rate in the meridional direction (primary flow direction) when computing the average. For this option to be available, the field functions Density and Cell Relative Velocity must be present in the simulation.

Average Profile Properties

Parameterization

Selects an axisymmetric parameterization that includes the input parts chosen for this derived part.

Binning Mode

Determines how to generate the 1D bins:

• Equal distance—you specify the number of bins, and all bins are of equal size.
• Mesh resolved—the bin size adjusts to half the local mesh size.

Note

A binning discrepancy has been observed between Linux and Windows, which can lead to slight differences in solution results between the two platforms for this derived part. Since the binning is very sensitive to any differences in values of either the coordinates of the geometry or the MSC (Meridional, Spanwise, Circumferential) field function values, you may get more or less bins on Linux as compared with Windows, causing shifts in the averaged values. Using the Equal distance option lessens this discrepancy.

Functions

Selects a field function with which to map back to the input surfaces. This property lets you produce a 1D data set of the circumferentially averaged solution on a given plane or surface. When you select an existing field function, for example Axial Velocity, for this property, a new field function appears, Average Profile: Axial Velocity. The circumferentially averaged field can be displayed on a 2D surface in the same shape as the input surface in order to examine it in context with the 3D model.

Consider the following when using this option:

• Adding or removing an Average Profile field function is only possible by selecting or deselecting its input field function in the Functions property.
• Deleting the input field function that was selected in the Functions property also deletes the corresponding Average Profile field function.
• An Average Profile field function may display invalid values on the input surfaces if it is partially mapped. An example would be mapping back from the average profile derived part to a part surface input of a boundary.

Weighting Mode

Determines whether and how to apply weighting as follows:

• Area—uses surface area only. For a field f, the averaged f is defined as:
  $$averaged{F}_i=\frac{\sum f_c{\mathbf{A}}_{\mathbf{ci}}}{\sum {\mathbf{A}}_{\mathbf{ci}}}$$

  Where subscript i is the bin index and c is the face index. ${\mathbf{A}}_{\mathbf{ci}}$ is the area of face c that overlaps within the ith bin.

• Area-Adjusted Scalar Function—multiplies the face area and a scalar of your choice by the face field function value when computing the average.
  $$averaged{F}_i=\frac{\sum {\phi }_c{f}_c{\mathbf{A}}_{\mathbf{ci}}}{\sum {\mathbf{A}}_{\mathbf{ci}}}$$

  Where ${\phi }_c$ is the chosen scalar field.

• Mass Flow—multiplies the face field function value by the mass flow rate in the meridional direction (primary flow direction) when computing the average.
  $${\dot{m}}_c={\rho }_c{\mathbf{v}}_{\mathbf{c}}·{\mathbf{A}}_{\mathbf{ci}}$$

  Where ${\rho }_c$ is the fluid density, ${\mathbf{v}}_{\mathbf{c}}$ is the fluid velocity at face c, and ${\mathbf{A}}_{\mathbf{ci}}$ is the directed area vector. In the context of turbomachinery, ${\mathbf{A}}_{\mathbf{ci}}$ would point along the u (streamwise/meridional) coordinate direction. Hence the averaging formula is given by:

  $$averaged{F}_i=\frac{\sum {massFlow}_c{f}_c}{\sum {\mathbf{A}}_{\mathbf{ci}}}$$

Subdivision Part Properties

Subdivision Mode

Selects the method by which to subdivide meshes.

Option	Activated Child Nodes
Parameters	Subdivision Parameters Provides a Base Level integer value for the number of subdivisions. Available values range from 0 to 5.
Field	Subdivision Field Lets you select a field function (in the property by that name) for the subdivision level. Available values range from 0 to 5. See Field Functions.

Point Probe Properties

Point

Specifies a Cartesian position vector that defines the location of the point.

Follow Motion

Controls whether the point probe moves together with a moving mesh or not. When activated, the point probe attaches itself to the moving mesh and keeps track of the cell it is in and its relative position within that cell. Every time the mesh moves, the point checks its position to ensure that it is inside the correct cell and in the correct position within that cell. When deactivated, the point probe remains stationary (assuming that its assigned coordinate system is not moving). This option works with all types of motion.

Highlight Input Coordinates

When activated, highlights the original coordinates that you specified, regardless of what happens to the corresponding point probe after intersection. For example, if a given point probe only has a volumetric region as its input part, that probe would exist only if it lies within the region. Otherwise it is invisible when Highlight Input Coordinates is deactivated.

This setting can help you check whether any of the points need modifications, such as transformation or scaling.

Line Probe Properties

Point 1

Specifies a Cartesian position vector defining one end of the line.

Point 2

Specifies a Cartesian position vector defining the other end of the line.

Resolution

Specifies the number of evenly spaced segments along the line. The actual number of points in the probe is one greater than the number of segments; fewer points may be generated if part of the probe lies outside the model geometry.

Presentation Grid Properties

Normal

Specifies the vector passing through the center of the presentation grid at a right-angle. Entering a new value for Normal automatically adjusts the values for Point 1, Point 2 and Origin, in order to define a grid that matches the current properties.. Use this property as an alternative to Point 1 and Point 2 to define the plane. You can include units in the entry, or select the units in the dialog that is activated by clicking (Custom Editor).

Origin

Specifies the lower-left corner on the presentation grid relative to the selected coordinate system. Entering a new value for Origin automatically adjusts the Normal, in order to define a grid that matches the current properties. You can include units in the entry, or select the units in the dialog that is activated by clicking (Custom Editor).

Point 1

Specifies the lower-right corner on the presentation grid, relative to the selected coordinate system. Entering a value for Point 1 automatically adjusts the Normal, in order to define a grid that matches the current properties. Use this property along with Point 2 as an alternative to Normal to define the plane. You can include units in the entry, or select the units in the dialog that is activated by clicking (Custom Editor).

Point 2

Specifies the upper-left corner on the presentation grid, relative to the selected coordinate system. Entering a new value for Point 2 automatically adjusts the Normal, in order to define a grid that matches the current properties. Use this property along with Point 1 as an alternative to Normal to define the plane. You can include units in the entry, or select the units in the dialog that is activated by clicking (Custom Editor).

X Resolution

Specifies the number of intervals between data points along the x-axis (that is, Number of Data Points = X Resolution + 1). The x-axis is the axis between the Origin and Point 1.

Y Resolution

Specifies the number of intervals between data points along the y-axis. The y-axis is the axis between the Origin and Point 2.

Arbitrary Probe Properties and Actions

Surface Input Option

Specifies the source of the input geometry. The available options are:

• File: allows you to read in points from a STL or VTK file.
• Part Surfaces: allows you to select one or more CAD part surfaces from which to extract the sample points.

Re-Import Data... (right-click action)

Allows you to load new sample points from an STL or VTK file.

Resampled Volume Properties

Origin

A Cartesian position vector that defines the origin of the resampled volume. You can include units in the entry, or select the units in the dialog that is activated by clicking (Custom Editor).

Rotation Axis

Sets the rotation axis for the resampled volume.

Size

Sets the size of the resampled volume in three dimensions. You can include units in the entry, or select the units in the dialog that is activated by clicking (Custom Editor).

Rotation Angle

Specifies the angle of rotation along the specified rotation axis in radians.

Cell Size to Voxel Ratio

Determines the discretization of the resulting structured voxel mesh. Increasing this value always increases the number of voxel cells. Based on two refinement metrics this value represents the ratio between the size of volume mesh cells and size of voxel cells. The size is defined by the chosen refinement metric:

• Values significantly lower than 1 lead to a down-sampling when comparing the number of volume mesh cells and number of voxel cells.
• Values around 1 lead to a more refined voxel mesh with a greater number of voxel cells.
• Values significantly above 1 are not recommended, because they can lead to unwanted over-refinement.

Refinement Metric

Allows an adjustment in the definition of the Cell Size to Voxel Ratio setting:

• Surface: uses the ratio between the surface of a volume mesh cell and the surface of a voxel cell.
• Diagonal: uses the diagonal of a hexahedral bounding box around a volume mesh cell.

  This option, which is the default, reduces the amount of voxels generated in portions of a model that contain prism layers and is therefore preferable to the Surface option.

Minimum Voxel Size

Sets the minimum size of a voxel cell. The minimum size is based on edge-length of the cubic voxel cell. No voxel with a length smaller than this value is created. The Minimum Voxel Size has precedence over the Cell Size to Voxel Ratio. For data structural reasons the minimal number of voxel cells cannot be smaller than 4913 voxels.

Resampled Volume Settings Properties

Rendering Mode

Allows you to select a mode of rendering. The following options are available:

• Volume - Every scalar sample value is mapped to the displayer opacity plus color, and is then attenuated along the view direction.
• Isosurface - Allows you to choose between single or multiple surfaces. Activates a Isosurface Mode sub-node.
• Maximum Opacity Projection - A transparent mode with high contrast to highlight volume areas that contain scalars with high opacity. An example is when velocity magnitude is mapped to a high-pass color map. The transparent mode reveals additional points of interest, regardless of the opacity attenuation which is depending on the viewpoint. However, the projective nature of this mode removes clues for depth perception.
• Plane Section - Allows you to incorporate interactive plane sections in the volume rendering. Activates a Plane Sections sub-node.

  If you activate the Display Mesh property of the displayer that includes these section planes, the planes show the mesh of the resampled volume itself, letting you view the size of individual voxels that are used to resample a field.

  
  
  

  To display the original grid, use a plane section derived part (instead of a resampled volume derived part).

Lighting Mode

Allows you to apply displayer lighting to the volume rendering. The primary application for the Local Lighting mode is when the Rendering Mode property is set to Isosurface. In the Isosurface mode, standard lighting is applied to the isosurface exactly as if it were a proper surface. Additionally, local lighting is used in the Volume rendering mode for a more “surface-like” image without actually reverting to simple surfaces.

• None - Does not use displayer lighting.
• Local Lighting - Applies the settings of the displayer surface lighting. The advantage of this technique is that details in the scalar field can be discerned more easily in many cases. The following Marschner-Lobb examples of volume rendering illustrate the benefit of local lighting.
  • Local lighting:
    
    
  • No local lighting:
    
    
• Automatic - By default, deactivates lighting effects for Volume and Maximum Opacity Projection rendering modes, and activates lighting effects for Isosurface and Plane Section rendering modes.

Quality

Determines how accurately the resampled volume is processed during ray-casting.

Volume Rendered Isosurface Mode Properties

Isosurface Mode

The mode for isosurface volume rendering, specifying whether a single surface or multiple surfaces are created.

• Single - Uses one surface (default).
• Multiple (range) - Selects a range technique for creating multiple surfaces.
• Multiple (arbitrary) - Selects an arbitrary technique for creating multiple surfaces.

Volume Rendered Plane Sections Object Properties

The Plane Sections node contains the volume rendered plane section objects in the displayer. Use the properties of any of these objects to activate it, deactivate it, and specify its coordinates.

Origin

Sets x, y, and z coordinates for the origin of the plane.

Normal

Sets x, y, and z coordinates for the second point of the plane.

Enabled

Uses a checkbox to turn the clip plane on or off.