8.1. Model Preparation

Model preparation includes all steps that are necessary to create a finite element model database and physics files for the generation pass. The following flowchart illustrates the process involved.

Figure 8.2:  Model Preparation Flowchart

Model Preparation Flowchart

Each step is explained in detail below:

8.1.1. Build the Solid Model

As a first step, you must build a solid model of the structure, and the electrostatic field surrounding the structure. To build the model, you must specify a jobname (for example, MODEL) using either of the following:

Command(s): /FILNAME
GUI: Utility Menu> File> Change Jobname

You use the PREP7 preprocessor to define the element types, element real constants, material properties, and the model geometry. For information on how to build a solid model, see Building the Model in the Basic Analysis Guide and Solid Modeling in the Modeling and Meshing Guide.

8.1.2. Mesh the Model

Once you have built your solid model, you are ready to generate the finite element mesh. For information on meshing techniques, see Generating the Mesh in the Modeling and Meshing Guide.

8.1.3. Create Structural Physics File

Next, you must create a structural physics file entitled “STRU” in accordance with the physics environment approach described in Load Transfer Coupled Physics Analysis. It must include material properties, real constants, fixed zero boundary conditions, and initial prestress conditions. Some important points to remember are:

  • Apply all zero-value displacement constraints to solid model entities.

  • Do not apply any nonzero displacement or nodal forces in the model database. These can be applied later during the use pass at specific master nodes.

  • Apply prestress conditions in the model database by means of thermal stress. Specify appropriate element temperatures and thermal expansion coefficients.

  • Do not apply element loads (pressure, or gravity loading) in the model database. These types of loads may be specified later in the Generation Pass.

  • Group nodes on which eigenmodes will be imposed during the generation pass into a node component called "NEUN.” Limit the number of nodes to 5000 minus the number of defined scalar parameters in the model. Select a distributed subset of the nodes on the neutral plane if this limit is exceeded.

  • In order to obtain a proper set of strain energy and capacitance information in the design space, the movable structure must be displaced to various linear combinations of their eigenmodes. Those deformation states are internally imposed by appropriate displacement constraints in the operating direction. In practice, it is unnecessary to impose displacement constraints on all structural nodes. It is sufficient to just choose nodes on a neutral plane of the structure, which is perpendicular to the operating direction. This allows the structure to relax properly and it is especially necessary for stress stiffened structures. If the device does not undergo stress stiffening, then any plane of nodes perpendicular to the operating direction may be selected.

You use either of the following to create the structural physics file (MODEL.ph1).

Command(s): PHYSICS,WRITE,STRU
GUI: Main Menu> Preprocessor> Physics> Environment

8.1.4. Create Electrostatic Physics File

Next, you must create an electrostatic physics file entitled “ELEC” in accordance with the physics environment approach described in Load Transfer Coupled Physics Analysis. It must include material properties and conductor specifications. Some important points to remember are:

  • Group nodes of each conductor into components "CONDi," where i is a successive number assigned to each conductor.

  • Group all volumes (3-D analysis) or all areas (2-D analysis) to be morphed or remeshed into a component called "AIR.”

  • Do not apply zero and nonzero voltage loads and imposed current to the model database. These excitations and boundary conditions can only be applied during the use pass.

You use either of the following to create the electrostatic physics file (MODEL.ph2).

Command(s): PHYSICS,WRITE,ELEC
GUI: Main Menu> Preprocessor> Physics> Environment

8.1.5. Save Model Database

At this point, you need to save your database for use in the rest of the ROM procedure. The file name defaults to the Jobname (MODEL).

Command(s): SAVE
GUI: Utility Menu>File>Save as Jobname.db

Release 18.2 - © ANSYS, Inc. All rights reserved.