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:
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), etc.
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.
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 equalt 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:Split the large assemblies into smaller (if possible, geometrically less-dependent) domain. This helps avoid large memory requirement and further geometry clean-up operations as well.
Step-2: Re-group and rename the dataThe geometry in CAD environment is created keeping in mind the physical construction and assembly sequences. This is not important in mesh generation. It is better to re-group the geometrical (CAD) entities in terms of expected boundry definition. This makes it easy to operate on a smaller section of the entire domain. The selection, hide/unhide and operations such as imprint/ interference become faster.
Step-3:Further segregate the geometry into 'Solids' and 'Surfaces'. This helps chose operations appropriate for the respective category. Such as fillet removal, split, booleans and extrude (pull) is easy on solids.
Step-4:Convert the solids with thin wall thickness into solids with no internal wall and void. For example, a beam with fillets and internal wall.
Step-5:Before removing the wall thicknesss, use the operations appropriate for solids such as Booleans like unite, intersect... to make sure the once converted to surface, no further operations such as extend /intersectio is needed to remove the gaps / connect the surfaces. Note that this method is no recommended for FEA simulation. in CFD the blockage of flow is important where as in FEA the location of centroid is important.
Step-5:ANSYS Spaceclaim is a CAD-type pre-processor and works better on solids. CFD volume extraction is a analogous to 'negative' of visible solid volumes. Instead of deleted the unwanted surfaces one-by-one, it is recommended and worth trying to create a "bounding box" enclosing the geometry and use a bolleaan to subtract the solids from the 'bounding' box. The resultant negative volume of fluid domain is easy to operate and remove the protrusions generated due to gaps in original (input) geometry.
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:
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.
Do not 'stitch' the geometry body and surfaces until you are dones 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.
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-ais 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).All the 3 examples above demonstrate the versatility of parametric representation of a curve. However, we need to always have a independent variable (u or θ) as parameter. Even, x or y or z themselves can be a parameter so that x=f(x), y=g(x) and z=h(x). Similarly, the surfaces can be represented parmetrically. This is the reason the 3D CAD geometry in SolidWorks, Unigraphics, Creo, Inventor, FreeCAD... are called parametric models and the method is called parametric modeling.
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 + c3u3The unique set of 12 constant coefficients are known as algebraic coefficients and determines the size, shape and position of the curve in space.
Geometric Form of a Parametric Cubic (PC) Curve: Algebraic coefficients do not lend much flexibility to control the shape of a curve in modeling 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.
Finally, p(u) = (2u3 - 3 u2 + 1) p(0) + (-2u3 + 3u2) p(1) + (u3 - 2u2 + u) p'(0) + (u3 - u2) p'(1).
The content on CFDyna.com is being constantly refined and improvised with on-the-job experience, testing, and training. Examples might be simplified to improve insight into the physics and basic understanding. Linked pages, articles, references, and examples are constantly reviewed to reduce errors, but we cannot warrant full correctness of all content.
Template by OS Templates