Chapter 1: Overview of Model Generation

Chapter 1 * Chapter 2 * Chapter 3 * Chapter 4 * Chapter 5 * Chapter 6 * Chapter 7 * Chapter 8 * Chapter 9 * Chapter 10 * Chapter 11 * Chapter 12 * Chapter 13 * Chapter 14

1.1 What Is Model Generation?

In ANSYS terminology, the term model generation usually takes on the narrower meaning of generating the nodes and elements that represent the spatial volume and connectivity of the actual system. Thus, model generation in this discussion will mean the process of defining the geometric configuration of the model's nodes and elements. The ANSYS program offers you the following approaches to model generation:

• Creating a solid model within ANSYS.
• Using direct generation.
• Importing a model created in a computer-aided design (CAD) system.

1.2 Typical Steps Involved in Model Generation Within ANSYS

• Begin by planning your approach. Determine your objectives, decide what basic form your model will take, choose appropriate element types, and consider how you will establish an appropriate mesh density. You will typically do this general planning before you initiate your ANSYS session.
• Enter the preprocessor (PREP7) to initiate your model-building session. Most often, you will build your model using solid modeling procedures.
• Establish a working plane.
• Generate basic geometric features using geometric primitives and Boolean operators.
• Activate the appropriate coordinate system.
• Generate other solid model features from the bottom up. That is, create keypoints, and then define lines, areas, and volumes as needed.
• Use more Boolean operators or number controls to join separate solid model regions together as appropriate.
• Create tables of element attributes (element types, real constants, material properties, and element coordinate systems).
• Set element attribute pointers.
• Set meshing controls to establish your desired mesh density if desired. This step is not always required because default element sizes exist when you enter the program (see Chapter 7). (If you want the program to refine the mesh automatically, exit the preprocessor at this point, and activate adaptive meshing.)
• Create nodes and elements by meshing your solid model.
• After you have generated nodes and elements, add features such as surface-to-surface contact elements, coupled degrees of freedom, and constraint equations.
• Save your model data to Jobname.DB.
• Exit the preprocessor.

1.2.1 Comparing Solid Modeling and Direct Generation

Although some automatic data generation is possible, the direct generation method is essentially a hands-on, "manual" method that requires you to keep track of all your node numbers as you develop your finite element mesh. This detailed bookkeeping can become tedious for large models, contributing to the potential for modeling errors. Solid modeling is usually more powerful and versatile than direct generation, and is commonly the preferred method for generating your model.

In spite of the many advantages of solid modeling, you might occasionally encounter circumstances where direct generation will be more useful. You can easily switch back and forth between direct generation and solid modeling, using the different techniques as appropriate to define different parts of your model.

Detailed discussions of solid modeling and direct generation can be found in Chapter 5 and Chapter 9, respectively. To help you judge which method might be more suitable for a given situation, the relative advantages and disadvantages of the two approaches are summarized here.

1.2.1.1 Solid Modeling

• Is generally more appropriate for large or complex models, especially 3-D models of solid volumes.
• Allows you to work with a relatively small number of data items.
• Allows geometric operations (such as dragging and rotations) that cannot be done with nodes and elements.
• Supports the use of "primitive" areas and volumes (such as polygonal areas and cylindrical volumes) and Boolean operations (intersections, subtractions, etc.) for "top down" construction of your model.
• Facilitates your use of the ANSYS program's design optimization features.
• Is required for adaptive meshing.
• Is required in order to do area mesh refinement after loads have been applied (solid model loads are also required).
• Readily allows modifications to geometry.
• Facilitates changes to element distribution; you are not bound to one analysis model.

• Can sometimes require large amounts of CPU time.
• Can (for small, simple models) sometimes be more cumbersome, requiring more data entries than direct generation.
• Can sometimes "fail" (the program will not be able to generate the finite element mesh) under certain circumstances.

1.2.1.2 Direct Generation

• Is convenient for small or simple models.
• Provides you with complete control over the geometry and numbering of every node and every element.

• Is usually too time consuming for all but the simplest models; the volume of data you must work with can become overwhelming.
• Cannot be used with adaptive meshing.
• Makes design optimization less convenient.
• Makes it difficult to modify the mesh (tools such as area mesh refinement, SmartSizing, etc. cannot be used).
• Can become tedious, requiring you to pay more attention to every detail of your mesh; tedium can sometimes cause you to become more prone to committing errors.

1.3 Importing Solid Models Created in CAD systems

• You can avoid a duplication of effort by using existing CAD models to generate solid models for analysis.
• Engineers can use familiar tools to create their models.

Go to the beginning of this chapter