Cross-learning: FLUENT / CFX / STAR-CCM+
Same concept - different approaches!
This page is intended to enhance the learning one CFD software to another by providing similarities and difference in approach. The purpose it to help user's learn new software when he/she is familiar with one, the purpose is not to rate any particular software.
Some definitions specific to STAR-CCM+
Continuum: Continuum is used to contain selections of physics or meshing models that are subsequently applied to one or more regions. Continuum have no geometric definition associated with it.
Mesh Continuum: A mesh continuum contains a selection of meshing models, such as the surface remesher, the prism layer mesher and the polyhedral mesher. When a mesh continuum is applied to a region, the region is discretized according to the meshing models selected for the mesh continuum. While using "Automated Mesh operation" to generate volume mesh, 'parts' must be assigned to 'regions'.
Physics Continuum: A physics continuum contains a selection of physics models, such as a chosen flow solver, material models, steady or transient time model, a turbulence model, and so on. Each physics continuum represents a single substance that is present in all regions to which the physics
continuum applies. Fluid Continuum and Solid continuum are two used to designate Fluid and Solid materials.
Model: Model nodes in the simulation object tree represent simulation features that are active in the current case. Model nodes are contained within the meshing and physics continua to control the construction of surface and volume meshes and physics models to define the behavior of the specified material.
Regions: Regions are volume domains (or areas in a two-dimensional case) in space that are completely surrounded by boundaries. They are not necessarily contiguous and can be linked to each other through interface type boundaries. Regions are created either when a volume mesh is imported or when a surface is imported without using geometry parts. Each region is given a unique name during the import process which can be renamed as per user's convenience.
Boundaries: Boundaries are surfaces (or lines in a two-dimensional case) that completely surround and define a region. Boundaries are never shared between regions - a boundary can belong to only one region.
Scene: A scene facilitate visual representation of the model
- Root ObjectThe root object within each simulation object tree is known as the simulation node. This node has its own properties and pop-up menu.
- Parts: There are three different types of part that can be used in a STAR-CCM+ simulation: Model parts (including regions, boundaries, and interfaces contained within the Regions, Boundaries, and Interfaces manager nodes - representing the discretized portions of the geometry to be analyzed, on which physics models are applied.
- Geometry parts (model geometry)
- Derived parts (parts used in the definition of analysis reports and for visualizing solution data in scalar and vector scenes.
Following table is an attempt to draw some similarities and analogies between various names and concepts used in CFD programs. However, there is no distinct boundaries and there are overlaps the way these designations refer to underlying objects and collectors.
The terms used in this table are building blocks of a simulation which consists of physical space (3D volume designated as domain or region), boundaries of a volume (known as surface regions or face zones), solver types (known as viscous model or continua) and so on. A generic term which can be used for all the objects mentioned in above table is 'collector' which is a collection or group of different physical (nodes, faces...) objects and numerical (turbulence model, material properties ...) objects. Few additional terms used to describe the computational volume are walls, interfaces and contacts.
|Identifier || STAR-CCM+ ||FLUENT || CFX ||OpenFOAM / ParaView |
|Solvers ||Physics Continua ||Viscous Model || - ||Application |
|Parts ||Mesh Continua || || Zones ||Boundary|
|Regions ||Continua ||Cell Zones, Face Zones || Cell Zones, Face Zones ||Blocks |
|Domains ||Continua ||Cell Zones, Face Zones || Cell Zones, Face Zones ||Blocks |
|Boundaries || ||Cell Zones, Face Zones || Face Zones, Edge Zones ||Boundary|
|Zones || Regions, boundaries || || ||Boundary, Patch|
|Case ||Model ||Case ||Definition ||Folder |
|Scenes || Separate for Geometry, Mesh, Scalar, Vector || Common for Scalar and Vectors, Planes || Common for Scalar and Vectors, Planes || Views and Filters: Render View, Slice View... |
Defining the Simulation Topology
Geometry is defined in terms of geometry volume, surfaces, curves and points. The discretized geometry is defined in terms of body points (volumes), faces, edges and nodes / vertices. The collection of these entities are designated as 'parts' in ICEM CFD, zones in "FLUENT", "regions and boundaries" in STAR CCM+ and "Assembly, Primitive 2D, Primitive 3D" in CFX. The computational model to which physics can be applied is defined in terms of regions (domains or zones defined in FLUENT, CFX) and boundaries. Defining the simulation topology is the process of mapping between the geometrical definition of the problem and the computational (or physical) definition.
In STAR CCM+, geometry parts refers to volume which can be assigned to regions, part surfaces can be assigned to boundaries, and part curves can be assigned to objects called feature curves. This mapping is important if all the operations, CAD import till simulation is performed inside STAR CCM+ environment. If mesh is generated out of STAR-CCM+ environment, these operations need to be performed in that application which will also write output file compatible to STAR-CCM+ requirements. For a typical CFD analysis, simple geometries are usually imported in CAD or non-CAD formats (or in more scientific terms, discrete or tessellated formats), while complex geometries usually come in mixed or hybrid formats, containing both CAD and non-CAD parts.
Difference in Descriptions
Most of the programs has keyboard short-cuts like famous control-c and control-v in MS-Windows OS. These are sometimes also called hot-keys. A summary of such keyboard features available in STAR-CCM+ are as follows:
- To align with the X-Y plane, press the 'T' key. Remember 'T' as initial of TOP view.
- To align with the Y-Z plane, press the 'F' key. Remember 'F as initial of FRONT view.
- To align with the Z-X plane, press the 'S' key. Remember 'S' as initial of SIDE view.
- To rotate the model about x-axis, press 'x' key. It will rotate 10° for every press of the 'x' key. Same if true for 'y' and'z' keys.
- To fit the view within the Graphics window, press the 'R' key.
- To rotate about the selected point, hold down the left mouse button and drag.
- To zoom in or out, hold down the middle mouse button and drag.
- To translate or pan, hold down the right mouse button and drag.
- To rotate around an axis perpendicular to the screen, press the 'Ctrl' key and hold down the left mouse button while dragging.
STAR-CCM+ Geometry Import
During geometry import, a choice of centimeters (cm), feet (ft), inches (in), kilometers (km), meters (m) (default), miles (mi), millimeters (mm), micrometers (um), and yards (yd) is allowed. The selection determines the scale factor that is applied to the import surface to make it conform to SI (meters). For example, selecting millimeters automatically scales the vertices by 0.001. If a unit other than one listed was used for the surface file, select the meters option (equivalent to no scaling). After the import process is complete, you can apply a user-defined scaling factor to scale the mesh.
If a unit other than meters (m) was selected, then the option to Set preferred units for length is available (off by default). This option can be used to set the selected unit as the default for all mesh reference and input values that involve length. Leaving the option off maintains meters as the default unit for length.
STAR-CCM+ Tools and Scenes
Software RecommendationsExcerpts from user manuals and tutorials for STAR-CCM+
There are two meshing approach in STAR: parts-based meshing and region-based meshing. Parts-based meshing approach is recommended, though one need not always follow this approach to generate a mesh. For simple geometry and assemblies consisting of few sub-assemblies, one can import parts, assign parts to regions, then generate mesh at the regions level. However, if while working with assemblies that contain tens or hundreds of parts, parts-based meshing approach is recommended.
STAR-CCM+ also includes a comprehensive set of surface-repair tools that allow users to interactively enhance the quality of imported or wrapped surfaces, offering the choice of a completely automatic repair, user control, or a combination of both. One of the most important elements of surface repair tool is its diagnostics tool. It offers functionality to identify error prone parts, surfaces and feature edges and provide real time information via the browse tool as you fix them.
Operations – utilities that perform actions on 'Parts', Certain operations such as "extract volume", "surface wrapper" ... create new parts.
STAR-CCM+ Mesh Checker
STAR-CCM+ allows to imprint parts non-conformally. This process is useful when:
- pierced faces: A pierced face is one that has one or more edges of another surface cell piercing it.
- poor quality faces:
- close proximity faces (surface folds and overlaps):
- free edges (holes and mismatched edges): Free edges refer to cell faces that are not connected to a neighboring face. free edges can be fixed by using the hole filler, the edge zipper, or the manual fixing tools, depending the nature of the problem. To repair click on the number on the Count list and all the problematic part would appear in pink. Then if it is for example problematic faces (that are overcreated) select them one by one or with ctrl or with the Zone selection tool and delete them. Then you will have to fill the holes you created with this action or the ones made by the software when importing the geometry.
- non-manifold edges: A non-manifold edge refers to a cell face edge that is connected to two (or more) other edges. A non-manifold edge is sometimes valid depending on whether the surface cells causing the problem are supposed to be a part of the geometry or not. For example, consider a geometry that contains a baffle surface that is joined to the exterior surface. This geometry is not a problem as long as the surface is converted to an interface before proceeding with the volume meshing. If the non-manifold edge is not expected, then you can delete the faces that are causing the problem.
- non-manifold vertices: Typically vertices connected to a surface instead of two or more edges.
- holes or leaks: Leaks are not desired because they cause an inversion in the wrapping process, which results in the incorrect volumes being wrapped. Run the leak detection tool to identify less obvious gaps and holes. The hole filler can be used to close any closed loop (both single and multiple loops) planar hole within a surface. The edge zipper can be used to join two mismatched surface edges that are within close proximity to one another, so that a closed surface is formed. Two different tools are available to help close off holes, namely the polygonal patch fill and the hole filler.
The polygonal patch filler is a quick and easy way of closing arbitrary shaped holes which do not have a closed loop definition and/or are not planar. The process literally 'patches' up the surface by creating faces that cover the hole area completely. Having an overlap in the patched surface is perfectly acceptable as the wrapper deals with this overlap automatically.
The hole filler is a more exact method of filling well-defined holes by using a closed loop feature edge definition around the hole.
- missing faces:
- duplicate faces -- surface repair -- Merge/Imprint: The tool also lets you merge two or more overlapping (co-planar) surfaces or sets of faces. When using Merge/Imprint on a single part, the result is either a common shared surface or no surface at all (that is, the common area is removed). If there are multiple parts, the tool creates part contacts for the shared surface. Similarly, for feature curves belonging to the same parts, the tool can imprint two or more edges onto each other, effectively zipping them together. You can also imprint edges onto faces and imprint faces onto edges, depending on the requirement. No edge options are available when imprinting across multiple parts. In all instances, the faces or edges do not need to belong to a closed surface in order to use the tool.
- Automatic repair tool can fix certain global surface problems that relate to bad quality, close proximity and/or intersections (pierced faces) at the push of a button. If you want to fill a large number of holes automatically or zip a large number of edges then you should use the hole filler and edge zipper tools respectively.
- Surface wrapping and partial wrapping: In addition to refining the surfaces of parts in the wrap, partial wrapping can be used to exclude selected parts or part surfaces from the wrap operation. Excluded parts from the wrap, the original tessellation of the those parts is passed through to the final wrap surface. Some geometries only require surface wrapping for a portion of their surface. The surface wrapper allows you to exclude part surfaces that you consider sufficiently well tessellated for subsequent mesh operations. In some cases wrapping the whole geometry is unnecessary and can defeature highly detailed part surfaces unless the surface wrapper is excessively refined using custom controls and contact preventions. Select the Geometry > Operations > Surface Wrapper node and activate the "Perform Partial Wrapping".
- Imprint is a process of making a common boundary between two volumes. If two square blocks are touching each other, there are two faces, one each belong to each square. When imprint is performed, the one of the common surface is deleted. The imprint operation will result into entity known as 'contacts' in STAR, and may become interfaces when parts are transferred to regions. Four types of contact definition exists: In-place, Weak in-place (meshed non-conformally), Periodic, Baffle. Part-part contacts may be created (a) automatically during geometry import, (b)by imprinting, (c)by tolerance based searching and (d)manually
- a conformal interface is not necessary to achieve solution accuracy
- there are many contacting parts
- each part is within many pairs
- there are gaps between the CAD parts
Contact Prevention When the clearance between two surfaces is less than the target surface size, use a contact prevention to tell the wrapper not to join the two boundaries. The Minimum Size value indicates the triangle size in the space between the two parts, which determines the octree refinement in the area. The value is smaller than the gap size (typically one half or one quarter of the distance). You can still join the surfaces even though a Minimum Size value is set. The Minimum Size value is simply a stopping size for the surface wrapper refinement, which results in the two surfaces being separated. The value also has to be greater than zero.
Non-conformal ImprintingDuring the process of non-conformal imprinting, pairs of split surfaces are created on contacting parts without altering the individual parts or creating shared faces. To achieve a non-conformal mesh when imprinting these surfaces, before you imprint the parts, activate Show Advanced Parameters and set Resulting Mesh Type to Non-Conformal. After imprinting the parts, the resultant surfaces are non-conformal, which means that the surface discretization on the imprinted surfaces does not match. Each part remains separate and there is no shared surface between each part. However, the original discretized surfaces are cut and a pair of split part surfaces are created which represent an in-place part contact between the surfaces.
Manual Surface PreparationThe manual surface preparation tools contained within STAR-CCM+ allow you to:
To capture the complex and intricate features of the geometry the mesh generation process utilizes contact prevention conditions, volumetric controls and the wrapper scale factor. Wrapped surface is then retriangulated using the surface remesher.
- diagnose and locate each surface issue
- delete faces and edges and create new ones
- collapse and smooth vertices
- fill and patch holes
- split and swap edges
- locally zip edges
- locally remesh faces (with or without feature retention)
- isolate connected surfaces and delete them if necessary
- inflate thin shell/baffle surfaces so that they have thickness
- translate a surface
FiltersSix basic repair filter types (or predicates) available to use are listed below. Filter predicates can be used individually to search for parts or pieces of geometry and/or can be compounded within a filter, using logical operators (AND, OR or PIPE) to provide additional control.
Per-part meshing feature of "surface wrapping" operation allows multiple disconnected parts to be wrapped separately. The Minimum Size value indicates the triangle size in the space between the two parts, which determines the octree refinement in the area. The value should be set smaller than the gap size (typically one half or one quarter of the distance). It is just a stopping size for the surface wrapper refinement, which results in the two surfaces being separated. Surface wrapping process steps:
- Part Name: Search for parts based on the presentation name
- Part Surface Name: Search for part surfaces based on the presentation name
- Area: Search for faces/surfaces based on the area
- Volume: Search for closed surfaces based on the volume
- Area/Volume Ratio: Search for closed surfaces based on the area/volume ratio
- Face Count: Search for faces/surfaces based on the face count
- Global surface wrap at part / component level
- Contact prevention for small clearances -> One Group Contact Prevention Set / Two Group Contact Prevention Set
- Local refinements neas gaps using "Surface Control"
- Perform "partial wrapping" to capture local features like baffles, channels...[Split surface by patches, Preserved Input Surfaces-> Select "Excluded Surfaces"]
Continua: Solver Setting
Mesh Quality Checks in STAR-CCM+
Face quality is a measure of similarity between a face and the ideal face shape which is an equilateral triangle. The surface diagnostics calculate face quality = "in-circle radius / circumcircle radius" x 2. For an equilaterl triangle, in-circle radius * 2 = circum-circle radius. Thus, face quality '0' is degenerate triangle and 1 is the ideal shape. Default value of poor element setting in STAR-CCM+ is 0.01. The other definition in STAR-CCM+ as used in Surface Remesher is that quality of a triangle = the ratio of the triangle face area to the area of an equilateral triangle that would exactly fit inside the circumcircle of the triangle. The default value for surface remesher is 0.05
Dihedral angle of an edge is the angle between its adjacent faces. Edges are considered invalid if they are free or non-manifold as a dihedral angle cannot be calculated for such edges.
Removing Invalid Cells tool allows to remove mesh cells from the volume mesh region definition based on one or more of the following 4 mesh criteria: Face Validity, Cell Quality, Volume Change and Contiguous Cells. STAR-CCM+ moves all the removed cells into a separate region that is not used in the analysis. Symmetry plane boundaries are automatically added to the neighboring cell faces of cells that have been removed, minimizing the impact of these removed areas on the solution. Cells that do not meet the provided criteria are moved into a new region called Cells deleted from [Region] where [Region] is the name of continuum which these deleted cells belong to.
- Polyhedral quality: This value refers to the cell quality of the polyhedral cells.
- Cell face validity: This value refers to the face validity of the cells.
- Cell orthogonality: This value refers to the angle between the normals of two faces in a cell that share an edge. The closer the cell edge angles are to 90 degrees, the more orthogonal the cell is.
- Cell skewness angle: This skewness measure is designed to reflect whether the cells on either side of a face are formed in such a way as to permit diffusion of quantities without these quantities becoming unbounded. The skewness angle the angle between the face area vector (face normal) and the vector
connecting the two cell centroids. Skewness angle = 0 indicates a perfectly orthogonal mesh. Variables that are stored at interior faces in STAR-CCM+ cannot be displayed and hence the worst skewness angle for all the faces of a cell are stored in that cell. Thus, two cells often have the same skewness angle corresponding to the face that they share. To reduce the impact on robustness, avoid skewness angles greater than 85° as reported in the
mesh diagnostics full report.
- Cell Quality: It describes relative geometric distribution of the cell centroids of the face neighbor cells and of the orientation of the cell faces which is specified as 'Orthogonality' in some programs such as ANSYS FLUENT. Generally, flat cells with highly non-orthogonal faces have a low cell quality. A cell with a quality of 1.0 is considered perfect.
- Cell volume ratio: This value refers to the volume change between neighboring cells.
- Boundary Skewness Angle: it is defined as the angle between the area vector and the vector connecting the cell centroid and the boundary face centroid. This angle is important since the dot product of these two vectors appears in a denominator in a component of the equation for diffusive fluxes at a boundary face. In turbulent flows where wall functions are used, the equation for diffusive fluxes at a boundary is not used to compute diffusion fluxes at walls, so boundary face skewness become less important. However, it is important for laminar flows and for heat transfer in solids. To reduce the impact on robustness, avoid boundary skewness angles greater than 85° as reported in the mesh diagnostics full report.
- Face Validity Cell Metric: It is an area-weighted measure of the correctness of the face normals relative to their attached cell centroid. A face validity of 1.0 means that all face normals are correctly pointing away from the cell centroid. Values < 1.0 mean that some of the cell faces have normals pointing inward towards the cell centroid indicating some form of concavity. Values < 0.5 signify a negative volume cell.
- Volume change metric: It describes the ratio of the volume of a cell to that of its largest neighbor. A value of 1.0 indicates that the cell has a volume equal to or higher than its neighbors. A large jump in volume from one cell to another can cause potential inaccuracies and instability in the solvers. Consider cells with a volume change value < 10-5 to be suspect and investigate these cells further.