Solution Domain

Geometry or computational domain for CFD simulation requires a water tight geometry with simplification to handle the mesh creation process. Solution of computational domain refers to 2D or 3D geometry in which fluid flow and/or heat transfer phenomena need to be solved. This is known as "ZONES" in FLUENT, "REGIONS" in STAR-CCM+ and "DOMAIN" in CFX. These are "volumes surrounded by closed surfaces(called boundaries)" in 3D and "areas closed by edges or lines (called boundaries)" in 2D. It is the mesh and nodes generated to define and represent the physical space mathematically. No geometrical information is associated with the solution domain.

The geometry creation for CFD can be accomplished by either of the following two methods:

• Create geometry in any CAD (Computer-Aided Design) software such as Unigraphics, Catia, Pro/E, Solidedge. The geometry information created so far is called to be in "Native CAD" format. This geometry should be translated to a Neutral format such as IGES, STEP, Parasolid. All Pre-processors available has build-in capacity to read (Import) CAD data in this format. Once the geometry is imported into the Pre-processor, defeature as per requirement.
• The second approach is to create geometry directly into the pre-processor. All commercial pre-processors has basic built-in features to create Geometrical Entities. We strongly recommend this approach for following two cases:
  • 2D simulation
  • When geometry is axisymmetric. In this case, one needs to create the 2D cross-section first and then extrude it by rotation. In ANSYS FLUENT, in the axisymmetric model the boundary conditions should be such that the centerline (where the radius reduces to zero) is an axis type instead of a symmetry type. The axis should the z-axis. Thus, for all 2D simulations, FLUENT expects geometry to be in XY-plane.
• One widely used term in numerical simulation is Topology. A precise explanation is provided by Georgios Balafas in his master's thesis for the Master of Science program in Computational Mechanics "Polyhedral Mesh Generation for CFD-Analysis of Complex Structures": The topology of a mesh is an abstraction of the geometric model, that provides unambiguous, shape independent information about the relation between the entities that form the mesh structure. To this end, a mesh database is used in order to store various-level attributes of entities of different dimensions. These typically include 0-D entities, referred to, in literature, as vertices or nodes, 1-D entities, referred to as edges, 2-D entities, referred to as faces or facets and 3-D entities, referred to as solids, volumes, regions or cells.
• Few other definition taken from previous reference:
  • "A face is said to be classified on the boundary of the geometric model, when it is adjacent to only one solid, which means that the free side of the face forms an external boundary. In the opposite case, where a face is adjacent to two solids, it is classified in the interior of the geometric model."
  • Mesh edges inherit their classification by their adjacent faces. Specifically, when an edge has at least one adjacent face that is classified on a model's boundary surface, the edge is also classified on the same boundary. To be more precise, in a conforming non-manifold three-dimensional mesh, an edge will have either zero or at least 2 adjacent boundary faces, however detecting one of them can be considered enough to classify the edge on the boundary as well. Furthermore, when an edge's adjacent boundary faces are classified on different boundary surfaces of the model, this denotes the edge's classification on a model's boundary edge, where 2 of its boundary surfaces intersect.
  • It is, therefore, adequate to count the amount of different boundary identifiers that are assigned to the adjacent faces of an edge, in order to conclude whether this edge is internal (zero boundary identifiers), on a boundary surface (one identifier), on a boundary edge (2 identifiers), or is a non-manifold edge (> 2 identifiers).
  • Extending the aforementioned classification criteria for vertices, a mesh vertex is classified on a model's boundary surface, when at least one of its adjacent edges is also classified on a boundary surface. Additionally, when at least one of the adjacent edges of a vertex is classified on a model's boundary edge, then the vertex is also classified on the same boundary edge. Finally, when there exist at least two adjacent edges classified on two different model's boundary edges, the vertex is classified on a model's corner, formed at the intersection of the boundary edges. In other words, the classification of a vertex with respect to the model can be determined by counting the amount of different boundary identifiers assigned to the adjacent faces of the vertex.
  • Zero boundary identifiers denote an internal vertex, while vertices on a boundary surface have adjacent faces with a unique identifier. Nodes on model's boundary edges have adjacency relationships to faces of two boundary identifiers in total and vertices on a model's corner sum up with three adjacent boundary identifiers. Finally, when a vertex has adjacent faces classified to more than three different boundary surfaces, the vertex is non-manifold.

Other operations include: extract centrelines (to plot variation of pressure or temperature vs. position), create mid-planes (to create plots on a non-planar surface), save curve data into .csv file, create enclosure, merges faces, create body-of-influence (BOI) geometry, create Face of Influence (FOI) geometry, scale-up or down a body... ANSYS Discovery has option to create Curve Tables and Hole Tables (Curve Table in the Annotation group under Detail tab), the centreline of a tube can be generated using 'Extract' tool in Beam section under Prepare tab. Fill Surface: create surfaces from free edges of a hole in a facet sheet body, Sew Sheet bodies: combine or sew multiple facet bodies into a single body, Bridge surface: (similar to loft operation in some CAD tools) create a body between two sets of edges of existing facet bodies. Extruding surfaces and sketches directly up to any user defined Plane with the "Up to Plane" method. Keep or delete imprinted edges when uniting bodies.

Creation of post-processing planes: when computational domain is not aligned to coordinate axes or the flow path are curved and twisted that any section would result in multiple non-contiguous surfaces, it is strongly recommended to create post-processing planes during geometry creation and meshing process. These faces should be named with prefix 'post_' and set as internal type in meshing (so that boundary layers do not grow over them). Though most of the solvers and post-processors has option to import such surfaces in STL format and imprint on the mesh, it is time consuming and may result in interpolation error. The 'internal' zone created shall have faces and nodes aligned on it and the solution variables are directly available there to calculate derived parameters such as mass flow rate and pressure. In case of imprinted surfaces, the solution variables have to be interpolated from nearest nodes, face and cell centers.

Unit Systems

All tools dealign with virtual geometry and mesh generation has option to scale the model. As units are not mentioned at every numerical value, scaling changes the value as per units specified. For example, for a cylinder the tool may contain information 'mm' in header row and only numbers for diameter, length and other keypoints (nodes, vertices...). When user changes the units to 'm', those values has to be divided by 1000 while only the header gets changed from 'mm' to 'm'.

Parametric Modeling (Geometry Creation) within CFD Environment

Parametric Modeling in ANSYS SpaceClaim / Discovery: For all operations which can be parametrized, the symbol 'P' in SpaceClaim and icon within context-menu in Discovery appear to create a parameter. The value field of a parameter can contain basic formula such as 0.02 * 25.4 to convert a dimension from inch to 'mm'.

Move operation is very much similar to Pull operation though the behaviour of the Move tool changes based on what is selected. If an entire object, such as a solid, surface, or sketch is selected, 'Move' operation translates or rotates the object. If one side of a solid, surface, or sketch is selected, move operation shall enlarge or reduce the size of the object. If an object is moved into another object in the same component, the smaller object is merged into the larger one and receives the larger object's properties. Moving the apex of a cone changes the height, Anchor the Move tool to the outer face to scale the cone.

Geometry Fully or Partially Enclosed in a Fluid Domain

It is not explicitly documented in SCDM user manual in which order the parameters get updated - however it is logical to assume that the parameters shall get updated in the order they are created / stored. And the parameters are stored in the order they are created and not in the order sorted by user say ascending alphabetically. It is better to define parameters with constant reference frame instead of taking reference from any other floating object.

Guidelines to Design Thermal Management System

1. The available space and envelope such as inlet and outlet connectors, location of fans... should be as per component placement
2. For gas (air) cooled systems:
   • The design approach with passive cooling (natural convection) and active cooling (forced convection) are different
   • Both may use heat spreader (heat sinks) and thermal interface material
   • In passive cooling, the orientation of the part and hence the orientation of heat spreader or heat sink should is along direction of gravity
   • For active cooling case, the location of fan should be inline with the heat sink and there should be diverging duct to control the swirl of the fans
3. For liquid cooled systems:
   • First criteria is to meet the pressure drop requirement (maximum permissible pressure drop) for specified flow rate
   • The cooling channel should be in a curved or serpentine shape to cover larger surface area which also ensures continuous mixing of hot and cold fluid (no formation of thermal boundary layer)
   • The heat conducting face of heat generating devices (MOSFET, IC, Capacitors...) should be directly mounted on the heat sink or cooling channel plates as per the layout of the components
   • Ensure good contact between the heat generating parts and the cooling plate or heat spreader by using thermal grease or thermal interface material (TIM)
   • The sizing of the channels are iterative: for cooling channels with Aluminium and copper, the liquid (cooling medium) velocity is limited to 2 [m/s] or 5-8 [ft/s]* and for stainless steel the limit is 4 [m/s]. This is to avoid pitting (erosion) at higher liquid velocities. High water velocity in copper channels can strip the protective copper oxide layers and thus accelerate corrosion-erosion of the channels
   • Sometimes a minimum average velocity is also need to be met to avoid fouling and depositions on the channel walls
   • The minimum wall thickness is governed by burst pressure requirements. In terms of thermal performance, a lower wall thickness leads to better conductive heat transfer.

Naming Convention of Boundaries and Cell Zones

1. Inlet(s) and outlet(s) should be named as b_inlet_id, b_outlet_id where 'id' stands for identifier.
2. Walls with boundary conditions (other than adiabatic): w_tpr_id, w_hfx_id, w_htc_id, w_rot_id w_mov_id, w_rgh_id, w_s2s_id where 'rgh' stands for rough walls, s2s stands for coupled solid walls.
3. Cell zones: fld_air_id, fld_wtr_id, fld_oil_id, fld_nnw_id, fld_rot_id, por_mom_id, por_thm_id, sld_alm_id, sld_stl_id, sld_src_id ... where 'nnw' stands for non-Newtonian fluids, 'src' stands for solid zones with heat source and/or sink and 'por' stands for porous (fluid) zones.
4. Internal planes: int_f2f_id, int_baf_id ... where 'baf' stands for thin walls or baffles.
5. Non-conformal interfaces: if_f2f_id, if_s2s_id, if_sta_rot_id, if_por_fld_id, if_por_por_id where 'sta' stands for 'stationary' zones and 'por' stands for 'porous' zones.
6. All boundaries with no special setting or conditions to be applied on them can be named as 'b_def_id' or dumy-id1, dumy-id2 or empt-id1, empt-id2 or fblk-id1, fblk-id2 where dumy stands for dummy, empt for empty and fblk for flow-blockers. This is especially important while dealing with assemblies with large number of solids and fluid zones.

A convenient frame of reference must be defined that applies to both model and prototype and corresponding locations must be defined using dimensionless ratios (for a sphere for example, angle on its surface, longitude and latitude lines). Thus, there exist similar conditions for corresponding points on both model and prototype. That is, the drag coefficient at a particular point on the sphere applies to both model and prototype.

The designer must follow, then geometric similarity (model and prototype), kinematic similarity (velocity vector direction is similar for both model and prototype), dynamic similarity (force vector direction is similar for both model and prototype), thermal similarity (heat fluxes)...

Note that similarity principles cannot be applied for all application without loss of accuracy. For example, to reduce size of an axial flow fan with shroud, either for numerical or experimental investigation, their is no thumb rule to account for blade-tip and shroud clearance. Hence, the designer has to establish his own "quality standards and acceptance criteria" to address this limitation

Domain size reduction by sub-modelling

Domain size reduction by axi-symmetry

Defeaturing in ANSYS Discovery

The pre-processing activities require geometry simplifications (defeaturing) and ANSYS SpaceClaim has some powerful non-parametric features. One of them is the 'Pull' option (short-cut 'p') which is equivalent to 'sweep' or 'extrude' operation. By default, pull direction is tangent to the selected edge or perpendicular to the selected face. A direction can be chosen or pulled (sweep) along a curve. Selection: all holes equal to selected radius, all holes of same radius in same face, all holes of radius equal or smaller than select radius. Blend (b): create surface by two lines (it is equivalent to 'loft' operation in some CAD programs). Fill (f): create surface from a closed loop of curves. Move (m): the 'origin' option is to select the reference point on the source object.

Step-by-Step for Geometry Defeaturing and Simplifications (ANSYS Spaceclaim)

Step-1:

Step-2: Re-group and rename the data

Step-3:

Step-4:

Step-5:

Step-5:

SpaceClaim has versatile feature called Pull operation which can be used to extrude faces and edges, create fillets and chamfer and remove materials. Tangent and Natural (curvature continuous) extension can be toggled when dragging the end of a curve. To drag the extension Tangent to the curve, press and hold Ctrl prior to dragging. Press 'Ctrl' and drag to 'Pull' the curve end tangent to the curve. Surface edges can be Pulled normal to their neighbouring face. Press the Ctrl key when you begin the Pull. Press Ctrl and drag to Pull the edge tangent to the surface. Pulling a face with its edges selected extrudes the face without influence from neighbouring faces. Pulling a conical face "Up To" a parallel cylindrical face replaces the cone with the cylinder if the axes are close together. Otherwise, the conical face is replaced with a cylindrical face that is coaxial to the cone and has the same radius as the cylinder.

Definition: gaps in the plane of a surface is called lateral (horizontal) gaps and gaps in the direction of area normal is called the transverse (vertical) gap.

If you are dealing with large surfaces with small (transverse) gaps (say < 1% of the biggest geometry or say 1-5 [mm] which you can neglect), follow these steps:

• Create a plane and/or planar surface encompassing the entire geometry which defines the best possible horizontal plane for the lower bound of the geometry.
• Extend (using 'extrude', 'sweep' or 'pull' tool) by amount which covers (fills) all the unevenness (transverse gaps) in the geometry.
• Split the bodies (solid volumes and surfaces) as per appropriate tool. E.g. in ANSYS SpaceClaim, "Split Body" can be used for both solid and surface bodies. 'Split' tool can be used for surfaces only.
• This process will remove the 'local' details such as 'openings', small surfaces or patches for named selection... Project the curves from original geometry as needed and then split the bigger surfaces created during previous operations.
• Delete the unwanted extensions created due to 'extend' and 'trim / split' operations.
• Repeat the process for other bodies in the assembly.
• Repeat the process for the upper and left / right bounds of the geometry. Though, once the lower and upper bounds are flattened (made coplanar), the 'blend' and 'fill' operation can be used to fill any lateral gaps between vertical edges and surfaces.

Fill operation: selecting many contiguous (connected) surfaces for fill operation does not work. However, selecting just one surface out of many makes the 'fill' tool act nicely. If 'fill' operation does not work while removing fillets and rounds, use Delete Rounds under Prepare > Remove > Rounds. Many a times, the sequence of fill operation determines the success of operation especially when fillets of different radii are connected in a loop. One need to visualize that the deletion of a fillet or blend should result in valid geometry.

Do not 'stitch' the geometry body and surfaces until you are done with all necessary clean-up and simplifications.

'Imprint' and 'Interference' operations do not make intended change in on go. Continue the operation till you get a message "No problem areas were fixed".

In ANSYS SpaceClaim, sometimes 'pull to' operation does not work. However, you can manually 'pull' or 'extend' the edges to or beyond the desired target edge. Hence, extend the edges manually and split them later to have a common boundary. Another option is to copy the surface(s) into a new model file and then do pull / fill / trim operations. Once desired shape is achieved, copy-paste the new geometry or shape back into main assembly.

Sometimes, the edges of the surfaces forming the gaps are short and split into many segments. Most of the geometry defeaturing programs have option to Fit Curves. However, this operation may not work if curves are already associated with surface. In ANSYS SpaceClaim, Patch Fill is another option. First click on Fill Ribbon tool without selecting any geometry. Under the options, the default is Extend Fill. Change the option to Patch Fill. If any geometry was previously selected, it would have extended fill.

Split Geometry for Meshing

ANSYS Discovery has option to save all the components into separate files. Select the components, right-click and chose Convert to External. The icon for the component in the Structure tree changes to indicate 'external'. A batch converter converter.exe located in the install directory of Discovery can be used to convert files to other formats.

If the bodies are stored without components, directly under root components, select the bodies which needs to be saved in separate files, right click and chose "Move Each to A Component". This will move each body in separate components and the steps mentioned earlier can now be used to save them into separate files. Discovery has different type of components: internal, external, dependent and independent.

How to compare two geometry when external appearance look similar? One way is to check the surface area - the one with higher value is expected to have bigger cross-section and lengths. This can be further confirmed by comparing the volumes of the two geometries.

Blender Tool for Geometry Clean-up

Other products offering similar features are Maya 3D and Houdini. From the website of Autodesk: "What is Maya? Maya is professional 3D software for creating realistic characters and blockbuster-worthy effects. Bring believable characters to life with engaging animation tools. Shape 3D objects and scenes with intuitive modelling tools. Create realistic effects – from explosions to cloth simulation." From the official page of Houdini: "Houdini is built from the ground up to be a procedural system that empowers artists to work freely, create multiple iterations and rapidly share workflows with colleagues. In Houdini, every action is stored in a node. These nodes are then “wired” into networks which define a “recipe” that can be tweaked to refine the outcome then repeated to create similar yet unique results. The ability for nodes to be saved and to pass information, in the form of attributes, down the chain is what gives Houdini its procedural nature."

Like many feature rich applications, the interface of Blender is a bit intimidating (complex and lost in ocean type) when you open it the first time. Understaing the GUI layout and context based sub-menu is key to get started.

Fix for Viewport Clipping

Some challenges dealign with tessellated geometries are removing fillets and chamfers from imported say STL file, deleting coincident surfaces (common boundaries of two closed volumes), removing proximities at sharp corners and point contacts such as a tire contacting flat ground.

ANSYS Discovery (known as SpaceClaim and DesignSpark) has on option called Vectorize Image that creates curves around colored areas in images. This can be used to create a 2D domain from images. A colour convention can be use to define domain and material types (solid, fluid, insulator...).

Curves

Linear parametric equation of curves: x = a + b.u, y = m + n.u, z = p + q.u where a, b, m, n, p and q are constants. The curves starts at p(u=0) = [a m p] and ends as [(a + b) (m + n) (p + q)] with direction cosines proportional to b, n and q.

Cubical parabola: x = a.u, y = b.u², z = c.u³ where a, b and c are constants.

Left-handed circular helix: Also known as machine screw, the curves are described as x = r.cos(u), y = r.sin(u), z = p.u where r and p are constants. It is the locus (path) of a point that revolves around the z-axis at radius r and moves parallel to the z-axis at a rate proportional to the angle of revolution 'u' (known as pitch of the helix). Note that if p < 0 then it is a right-handed screw (helix).

Algebraic Form of a Parametric Cubic (PC) Curve: Following 3 polynomials are required to define any curve segment of a PC curve:

x(u) = a₀ + a₁u + a₂u² + a₃u³

y(u) = b₀ + b₁u + b₂u² + b₃u³

z(u) = c₀ + c₁u + c₂u² + c₃u³

Geometric Form of a Parametric Cubic (PC) Curve: Algebraic coefficients do not lend much flexibility to control the shape of a curve in modelling situations as they do not account for conditions as its ends points or boundaries. When a curve is described based on its conditions as the ends (such as end point coordinates, tangents, curvature, torsion...), it is called geometric form of the curve.

STEP/IGES

Create Periodic Planes

The easiest option is to cut the geometry with two planes inclined at desired sector angle and passing through the axis of rotation. This option any cut through the blades (rotating as well as stationary) through the domain shall still remain periodic by definition.

Another approach is to draw a plane passing between two adjacent blades, the plane need not pass through exactly middle point of the leading edges. Create another plane inclined to the first plane at required sector angle. Split the geometry by these planes.

The following method is similar to previous one except 5 to 8 planes may be required to split the geometry into axial and tangential directions.

CAD Data Exchange

Similarly, to define 'names' in PTC Creo, the design can use: File > Prepare > Open Model Properties, then select 'Names' in the model properties dialogue. Then select faces by clicking > enter a name in the dialogue box opened in previous step. During CAD export to STEP format with default settings, the 'names' defined earlier do not get stored in the file. Change the export setup through File > Options > Configuration Editor > intf_out_assign_names > set it to 'user_name'.