When you create or import a geometric model into Patran, your primary goal is to produce a model which can be used for finite element analysis. The following sections describe some requirements for effective geometric modeling and suggest ways to verify that your model meets those requirements.

Topological congruency is a prerequisite for creating a valid finite element mesh because it assures that all regions of the model’s geometry can be made into one connected entity during the meshing process, so that it can be analyzed. To be topologically congruent, your model must meet the following requirements:

The following illustration shows an example of congruent geometry.

When edges of adjacent geometric regions are congruent (i.e., they match exactly), their meshes normally have the same number of nodes along common edges. In addition, the nodes along common edges are coincident; that is, they line up in pairs at the same locations along the common boundaries of the geometric regions. This includes matching pairs of corner nodes, or vertices.

During the equivalencing phase of the meshing process, these pairs of coincident nodes along the boundaries of the geometric regions are sewn together, so that the separate regions of the geometry form one connected entity that is ready to be analyzed.

The Geometry form selections Verify/Surface/Boundary and Verify/Solid/B-rep help you to locate areas of your model that are topologically incongruent. The Update Graphics form appears after you press Apply on the Geometry form. This form allows you to plot incongruent surfaces within a model.

The following figure shows two examples of incongruent geometry.

You may be able to get a consistent mesh for the leftmost surface if the edge of region 1 has exactly twice the number of elements as region 2 and region 3, and the mesh spacing is uniform. In this case the nodes could be equivalenced. However, if this surface were then remeshed--for example, with a specific mesh seed applied to one of these interior boundary edges--this would probably yield a mesh that could not be equivalenced.

In addition, if point 10 is not precisely in the center, the meshes for regions 1, 2, and 3 would not be likely to equivalence. Without equivalencing, these regions remain independent and unconnected. To make this surface congruent, choose either:

The surface on the right half of the previous figure shows a gap between two pairs of surfaces that is greater than the Global Model Tolerance. This means when you mesh the surface pairs, coincident nodes will not be created along both sides of the gap. To make this surface congruent, choose one of the following actions:

Try to keep the inside corners of the surfaces to 45 degrees or more. The reason is that when you mesh surfaces with quadrilateral elements, the shapes of the elements are determined by the overall shape of the surface. The more skewed the quadrilateral elements are, the less reasonable your analysis results might be. (For further recommendations, please consult the vendor documentation for your finite element analysis code.)

The direction of the out-of-plane normal vector of a surface is an important consideration for applying analysis data such as loads, boundary conditions, and element properties. In general, try to maintain the same normal direction for all surfaces in a model. The following figure shows opposing normals for two surfaces.

Use the Geometry application’s Edit/Surface/Reverse form to display the surface normal vectors, and to reverse or align the normals for a group of surfaces. This form has a button labeled Draw Normal Vectors that displays the positive surface normal vectors within your display. Alternatively, the Show/Surface/Attributes form can be used to display these normals.

You can also verify normals indirectly while constructing a surface, by displaying the parametric directions of the surface. To do this, choose Display /Geometry from the Main menu, select the Show Parametric Direction toggle, and then press Apply. These parametric directions will be displayed as lines at the parametric origin, labeled 1 and 2. The surface normal can be determined from these directions using what is known as the "right hand rule"--positioning your right hand so your fingers curl from axis 1 towards axis 2, the thumb pointing in the normal direction.

Put another way, the cross product of these two parametric axes produces a vector in the surface normal direction. To reverse the normal direction of a surface, use the Edit/Surface/Reverse form discussed above. This form allows you to select one or more surfaces, and reverses their normals by reversing their C1 and C2 parametric directions.

Beyond these basic criteria, some of the other goals in using Patran's geometric modeling in Patran include creating regions that mesh easily, contain separate regions as needed for the assignment of material and element properties, and contain features that facilitate the assignment of loads and boundary conditions.

To facilitate these goals, Patran contains numerous features for operating on existing geometry to simplify its analysis (for example, options to subdivide geometry into multiple regions, to work in multiple coordinate frames, and to use construction operations such as intersection and projection).

Above all, a geometric model in Patran is meant to be interacted with--an analysis of your model not only provides verification of whether it meets your design criteria, but also yields valuable feedback which can be used to further improve this design. You can then perform subsequent analyses to verify these changes.

This iterative cycle of adaptive analysis and design modification is central to the value of automated design analysis tools such as Patran, and it underscores the importance of using its geometric modeling features as a means of improving an existing design.