Browsers supply a great deal of view-related functionality by listing the parts of a model in a tabular and/or tree-based
format, and providing controls inside the table that allow you to alter the display of model parts.

FE geometry is topology on top of mesh, meaning CAD and mesh exist as a single entity. The purpose of FE geometry
is to add vertices, edges, surfaces, and solids on FE models which have no CAD geometry.

Many of the methods to check and edit mesh are based around determining mesh quality, but others check for mesh penetration,
detect holes, and locate edges or features.

Use the Normals tool to display and reverse the normals of elements or surfaces. The orientation of element normals can also be adjusted.
The normal of an element is determined by following the order of nodes of the element using the right-hand rule.

The quality of elements in a mesh can be gauged in many ways, and the methods used often depend not only on the element
type, but also on the individual solver used.

HyperWorks includes some alternate methods of calculating certain element types, which only apply to quads or rectangular faces
of solids, and only include alternate checks for Aspect Ratio, Skew, Taper and Warpage.

For the most part, OptiStruct uses the same checks as HyperMesh. However, OptiStruct uses its own method of calculating Aspect Ratio, and it does not support 3D element checks.

Use the Criteria legend to investigate the model via individual criteria and view a breakdown of all failed and worst
elements based on a set QI range. This is useful when you want to resolve criteria violations and evaluate the overall
quality of a mesh.

Use the Replicate tool to replicate a mesh from one location to another, with options to keep the original mesh, as
well as to replicate into multiple copies. The replicated elements replace the original elements, maintaining relevant
information like properties, thicknesses, and other solver attributes.

Locally refine 2D elements and attached 1D elements using either the Auto Quads tool, the Box tool, or the Manual tool. These are most useful for aerospace and marine applications, where specific transition patterns are required
from the refined mesh to the existing mesh.

Use the Detach tool to detach elements from the surrounding structure. You can detach elements from a portion of your model so that
it can be translated or moved, or you can offset the new nodes by a specified value. You can also use this panel
to detach and remove elements from your model.

Use the Imprint/Extend tool to extend a mesh to meet another mesh and form a good connection between them, or to imprint overlapping meshes
so that they match one another.

The Solid Mesh Optimization tool can be used to improve the quality of a tetra, hexas, and second order meshes with
respect to several element criteria.

Associate nodes to a point, line, or surface/solid face; move nodes along a surface; place a node at a point on a
surface; remap a list of nodes to a line; or project nodes to an imaginary line passing through two nodes.

Use the Split panel to split plates or solid elements. In addition, hexa elements can also be split using a technique
that moves progressively through a row of elements in the model

Stitch two unconnected meshes by adding elements between them, split elements at weld locations, and combine and split
elements to fix connectivity in the transitional area between fine and coarse mesh areas.

Perform a model-based CAD-CAD, CAD-FE or FE-FE comparison between two models, or two selections of entities, and find
and report geometrical/shape differences.

Tools and workflows that are dedicated to rapidly creating new parts for specific use cases, or amending existing
parts. The current capabilities are focused on stiffening parts.

Many of the methods to check and edit mesh are based around determining mesh quality, but others check for mesh penetration,
detect holes, and locate edges or features.

The quality of elements in a mesh can be gauged in many ways, and the methods used often depend not only on the element
type, but also on the individual solver used.

ANSYS-specific checks used to calculate element quality
for 2D and 3D elements.

2D and 3D Element Checks

These checks apply to both types of elements, but when applied to 3D elements they
are generally applied to each face of the element. The value of the worst face is
reported as the 3D element’s overall quality value.

Additional element checks not listed here are not part of the solver’s normal set of
checks, and therefore use HyperMesh check methods.

Aspect Ratio (tria)

For tria elements, a line is drawn from one node to the midpoint of the
opposite edge. Next, another line is drawn between the midpoints of the
remaining two sides. These lines are typically not perpendicular to each
other or to any of the element edges, but provide four points (three
midpoints plus the vertex).

Then, a rectangle is created for each of these two lines, such that one
line perpendicularly meets the midpoints of two opposing edges of the
rectangle, and the remaining edges of the rectangle pass through the end
points of the remaining line. This results in two rectangles, one
perpendicular to each of the two lines.

Third, this process is repeated for each of the remaining two nodes of
the tria element, resulting in the construction of four additional
rectangles (six in total).

Finally, each rectangle is examined to find the ratio of its longest
side to its shortest side. Of these six values—one for each
rectangle—the most extreme value is then divided by the square root of
three to produce the tria aspect ratio.

The best aspect ratio (an equilateral tria) is 1. Higher numbers
indicate greater deviation from equilateral.

Aspect Ratio (quad)

If the element is not flat, it’s projected to a plane which is based on
the average of the element’s corner normals. All subsequent calculations
are based on this projected element rather than the original (curved)
element.

Next, two lines are created which bisect opposite edges of the element.
These lines are typically not perpendicular to each other or to any of
the element edges, but they provide four midpoints.

Third, a rectangle is created for each line, such that the line
perpendicularly bisects two opposing edges of the created rectangle, and
the remaining two edges of the rectangle pass through the remaining
line’s endpoints. This creates two rectangles—one perpendicular to each
line.

Finally, the rectangles are compared to find the one with the greatest
length ratio of longest side to shortest side. This value is reported as
the quad’s aspect ratio. A value of one indicates a perfectly
equilateral element, while higher numbers indicate increasingly greater
deviation from equilateral.

Interior Angles

Maximum and minimum values are evaluated independently for triangles and
quadrilaterals.

Jacobian

Deviation of an element from its ideal or "perfect" shape, such as a
triangle’s deviation from equilateral. The Jacobian value ranges from
0.0 to 1.0, where 1.0 represents a perfectly shaped element. The
determinant of the Jacobian relates the local stretching of the
parametric space which is required to fit it onto the global coordinate
space.

HyperWorks evaluates the determinant of the Jacobian
matrix at each of the element’s integration points, also called Gauss
points, or at the element’s corner nodes, and reports the ratio between
the smallest and the largest. In the case of Jacobian evaluation at the
Gauss points, values of 0.7 and above are generally acceptable. You can
select which method of evaluation to use (Gauss point or corner node)
from the Check Element settings.

Length (min)

Minimum element lengths are calculated using one of two methods:

The shortest edge of the element. This method is used for
non-tetrahedral 3D elements.

The shortest distance from a corner node to its opposing edge
(or face, in the case of tetra elements); referred to as
"minimal normalized height".

Angle Deviation (Skew)

Only applicable to quadrilateral elements, and relies upon the angles
between adjacent legs at each corner node (that is, the interior angles
at each corner). Each angle is compared to a base of 90 degrees, and the
one with the largest deviation from 90 is reported as the angle
deviation. Triangular elements are given a value of zero.

Warping Factor

Only applicable to quadrilateral elements as well as the quadrilateral
faces of 3D bricks, wedges, and pyramids.

Calculated by creating a normal from the vector product of the element’s
two diagonals. Next, the element’s area is projected to a plane through
the average normal. Finally, the difference in height is measured
between each node of the original element and its corresponding node on
the projection. For flat elements, this is always zero, but for warped
elements one or more nodes will deviate from the plane. The greater the
difference, the more warped the element is.

The warping factor is calculated as the edge height difference divided
by the square root of the projected area.

3D Element Only Checks

ANSYS does not use any exclusively 3D checks within
HyperWorks, but HyperWorks does use its own
when ANSYS is set as the solver. For details on 3D
checks, refer to HyperMesh.