A Comprehensive Tool for the Assessment and Documentation of Finite Element Models

Developed by: CAEG, Inc.

Applicability: ANSYS^â Structural models, ANSYS 9.0

ANSYS is a registered trademark of ANSYS, Inc.

All other products mentioned in this document are

trademarks of their respective manufacturers.

Introduction

ModelChecker (MC) is a very versatile productivity tool that provides detailed information about any structural finite element model stored in the ANSYS^â database. Developed by Computer Aided Engineering Group (CAEG), this module is seamlessly integrated into the ANSYS^â Graphical User Interface and provides comprehensive assessment and documentation of the model attributes, boundary conditions, loads, and virtually all nonlinear and load step settings that exist. Furthermore, MC evaluates these settings for appropriateness. MC is designed to identify problems in the model and hence minimize unnecessary solutions, reduce model-debugging time, and most importantly, eliminate analysis runs that may produce incorrect solutions. MC automatically produces an HTML report containing the complete model description and assessment. This report can be personalized and customized to suit the user’s or the organization’s preferences.

MC is a collaborative tool that facilitates communication, review, and support of finite element models within organizations employing the ANSYS^â software. It can be a timesaving tool for beginners to FEA and a trouble-shooting tool for experienced analysts. For companies that distribute or outsource their computer aided engineering simulation, the use of MC and the resulting HTML report can provide critical finite element analysis (FEA) information to anyone in your organization, anywhere in the world, with Internet access.

MC can be easily installed on any computer platform including all UNIX and Windows networked systems or standalone installations. There are no compiler requirements or installation language prerequisites. Please refer to the section Installing ModelChecker for proper placement of the module granule and macro components.

The module appears as a menu selection in the Main menu of the ANSYS^â Graphical User interface when the user employs either the new interface (introduced at ANSYS^â 6.1) or the prior interface. Subsequent Dialog boxes allow you to select your desired model evaluation checks. The available selections will be discussed in the Model Checking Options section of this manual.

Objective

The objective of MC is to provide an in depth evaluation of your finite element model and an assessment of the model settings and loadings. MC was written by practicing finite element specialists of CAEG with over fifty years experience in providing ANSYS^â customer support, solving practical problems and providing ANSYS^â-specific and general finite element best practices education.

We have made our best efforts to provide you with accurate information when using MC. However, no software program is infallible and, as always, the user is ultimately responsible for final model checking. For more information about possible errors in MC and technical support please refer to the section: Incorrect Summaries from ModelChecker.

Overview

ModelChecker – What does this software do?

It provides a menu-driven (or batch), automatic, comprehensive assessment and documentation of any ANSYS^â structural model before the model is analyzed or solved. MC applies objective standards that can be customized and applied universally by organizations. The benefits over human checking are that it provides a thorough detailed check of every model, it has no biases, doesn’t tire from the tedium required to review a large number of details, and is very cost effective.

ModelChecker – Why should I use it?

· To thoroughly document the model

· To increase the reliability of all models, guarantees that every model has been reviewed/checked at a rigorous level

· To decrease the model debugging effort

· To minimize the number of solutions that produce incorrect results

· To minimize the number of solution runs

· To ensure there are no gross modeling mistakes

· To evaluate outsourced models

· To exchange FE model information anywhere, worldwide

· To minimize the support burden that inexperienced users place on expert users

· To educate inexperienced users in the creation of correct models

ModelChecker – When do I use it?

You can use MC at any time, interactively, during the modeling process. You may also elect to run MC in batch mode, perhaps in the final model verification stage. The software is completely flexible and can be used repeatedly as a debugging tool for certain iterative modeling functions, such as meshing. You may want to use it sequentially to provide information about the solid model, the element and attribute settings, the quality of the finite element mesh, and the applicability of the types of loadings and solver settings. In general, you will obtain the most benefit by using MC during and after model building.

This is not like a CAD import tool that is used only once on a given model! The whole idea is to find errors early in the process! If you wait till the end, run the checks and find out there is a mesh compatibility problem, much of the modeling work will have to be redone.

ModelChecker – What features of ANSYS^â are supported?

All current structural element types, their key options, all materials (linear and nonlinear), real or geometric constants, all nonlinear geometric and contact behavior, all special forms of model attachment using constraint equations and coupling, all possible applied loads and boundary conditions, and virtually all solution settings are considered.

ModelChecker – What hardware platforms are supported?

MC appears in the ANSYS^â graphical user interface as a Main Menu selection and, therefore, runs on all the ANSYS^â supported hardware platforms.

ModelChecker – What ANSYS^â products are supported?

MC can be used with ANSYS^â /Mechanical, Structural or Multiphysics. MC can be used with ANSYS^â /Professional and ANSYS^â /PrepPost but load and mass summaries cannot be done with either product.

ModelChecker – What type of results or output does it produce?

MC issues a comprehensive HTML report that can be viewed using any Web browser. The HTML report can be personalized and customized to suit the user’s preference. This report is written to a directory named JOBNAME_RPT (where “JOBNAME” is the jobname of your current session). This directory is located below the user’s working directory.

If MC is run interactively, the report is automatically displayed in your browser. If you do not want the report to be automatically displayed, define the value of the parameter, _caegshrpt=1, before MC is

invoked.

Note: The jobname portion of the HTML report filename and directory name will be truncated to the first 23 characters if the actual jobname has a longer name.

ModelChecker – Does it change or correct my model?

MC is a diagnostic tool, not a repair tool. In addition to the HTML report MC creates components that are intended to streamline error identification and correction by the user. MC does not attempt to change any features of the model that are causing warnings. In some cases, the warnings simply alert/remind the user of model characteristics that were actually intended and that are not real modeling errors or causes of concern.

Users are expected to make a backup copy of their database before running their models through MC. MC attempts to leave the database unchanged, except for the creation of parameters and components. MC also changes the jobname to caegrpt at the start of checking to ensure that no other jobname-related files (e.g., .esav, .emat files) are overwritten during checking. At the end of checking, the original jobname is restored. However, there is always the possibility that an inadvertent change could occur. MC must modify and then restore certain aspects of the model if any of the following combinations of checks and database characteristics are present.

• Load and/or mass summary is requested, MC issues the command KBC,1 to step the boundary conditions and hence ensure that the reported loads are the loads at the end of the load step. If spin softening is activated (see OMEGA command), it is deactivated. After the load and mass summary, KBC and the spin softening key are reset to their initial values.

• Thermal loads (temperatures) are applied to the model and load or mass summary is requested, MC writes the material properties to a file using the command MPWRITE, deletes the coefficients of thermal expansion (ALPX, etc.), runs the load and mass summaries, and then restores the original material properties (from the file) using the command MPREAD. This avoids the possibility of very small, spurious thermal loads (which should balance exactly to zero) in the load summary.

• Unsupported element types (by MC) are in the database and a load or mass summary is requested, MC sets these element types to NULL (element type 0), runs the load and mass summary, and then reissues the required ET commands to redefine the original element types and their key options. This modification is needed because errors have been discovered in the MC (not ANSYS^â) structural loads and masses when such element types are contained in the database.

If you intend to use the same database (used by MC) for your analysis, by all means double-check these items. In general, we recommend (we also wear belts and suspenders) that you make any required changes to the model using the backup copy of the database (not used by MC), this is the only method that ensures that MC has not, inadvertently, caused any model changes.

ModelChecker – Can ModelChecker be customized?

There are several variables (known as ANSYS^â parameters) that have been made available for customization. These variables can be used to:

1. control certain checking tolerances (such as coupling node coincidence).

2. limit the amount of model diagnostic information listed in the HTML report.

3. retain detailed model information (in arrays) not included in the HTML report that can be used for further model debugging.

These variables are discussed throughout this manual and detailed further in Appendix B.

Note: MC creates user-defined parametric variables and other variables during the model check. All variable names created by MC, with eight exceptions, begin with the “_” character. The eight exceptions are the arrays caegaar_, caegsc_, caegch_, caegkan_, caegms_, caegcap_,caeglli_, and caegls_. These array variables contain most of the model, mass, solid model, load information and plot captions. If MC defines a parameter that is currently defined in the model database, it will be overwritten. To list the currently defined underscore variables, in the ANSYS^â Input Window, type the command *STATUS, _prm. Users should avoid the use of such parameter names. MC also defines components with names beginning with “caeg”. Users should also avoid naming components or assemblies beginning with the letters “caeg”.

Getting Started

To utilize MC you must be a licensed user of the MC software and be running the current ANSYS^â release, ANSYS 9.0. Your evaluation of any structural model begins by resuming the model’s database or reading in an input file. MC will evaluate the model currently loaded/resident in computer memory. Therefore, if you are using load step files, you need to read the load data (for the load step being checked) into the database. To check your model select Model Checker™ from the ANSYS^â Main menu and proceed to identify the desired level of evaluation as guided by the ensuing Dialog boxes.

Interactive Execution of ANSYS^â and MC

Step 1: Start ANSYS^â interactively and activate your model

Utility Menu > File > Resume Jobname.db

Or: Resume from …

Or: Read Input from …

Note: MC works with either the old or the new ANSYS^â Menu System introduced at ANSYS 6.1 – the new menu is used as the default in current versions. The ANSYS^â menu system is also known as the Graphical User Interface.

MC does not work with the ANSYS^â Workbench Environment introduced at 7.0. The current ANSYS^â Workbench Environment does not provide access to all the functionality of ANSYS.

Step 2: Select the MC Module

Main Menu > ModelChecker(tm)

Step 3: Select the desired level of checking

MC Dialog Boxes and Run Interactive in the final dialog box

Note: Upon completion of the checks the HTML report is automatically displayed in your browser. If you do not want the report to come up automatically, set _caegshrpt=1 before running MC. See Appendix B for other user-defined variables.

Batch Execution of ANSYS^â and MC

Step 1: Start ANSYS^â interactively in the directory where the batch run will be made and establish the jobname for the MC batch run

Utility Menu > File > Change Jobname …

Step 2: Activate your model

Utility Menu > File > Resume Jobname.db

Or: Resume from …

Or: Read Input from …

Step 3: Select the desired level of checking

MC Dialog Boxes and Write Batch File in the final dialog box

This creates the batch input file caegbat.inp, which contains a RESUME command and all the required commands to invoke and run MC with the options that were chosen. It also creates the file caegrpt.ans (required to write the HTML report), which must remain in this directory until the batch run, is completed.

Step 4: Save your database for use in the batch model check

Issue the command SAVE

or

File > Exit > Save Geometry and Loads

Do not make any modifications to the database file (after writing the batch input files) as such changes could invalidate some of the earlier menu choices.

Step 5: Run the batch job using the file caegbat.inp as the input file and using the same jobname and working directory as used in the interactive setup.

If the batch job is to be run in another directory, the user must be sure to copy the files caegbat.inp, caegrpt.ans and the database to the new directory.

Note: MC batch runs will terminate when an ANSYS^â error is generated during checking and hence an HTML report will not be created. In such instances, please review the error file (caegrpt.err) to determine the nature of the error or evaluate your model using the MC interactive procedure described above.

Using ModelChecker Efficiently

Here are some guidelines to gain the most efficiency from MC.

• Check only what is currently defined for the model. If certain items haven’t been defined on the model there is no reason to check such items, i.e., don’t ask for a load summary if you haven’t defined any loading.

• Use the ANSYS^â select logic to limit the portions of the solid model and FEA model being checked. In general, most of the checks are only performed on the selected entities. To ensure that a consistent set of finite element entities is selected, MC starts by automatically selecting the nodes associated with the selected elements.

• If both the solid model and finite element model are present, be sure that you have a consistent selection of both types of entities before requesting a model check. MC automatically transfers solid model boundary conditions to the FEA model during checking. The selected solid model entities and selected FEA model entities will determine what boundary conditions, if any, will be transferred.

• Delay all, or most, model plot requests until all warnings and errors are resolved. The plot options allow the user to easily request many plots. On large 3-D models, the ANSYS^â plotting time can easily exceed the time required to check the model and hence slow the checking process.

• Avoid large assigned number disparities in your model (e.g., only two nodes in the model, but they are numbered 1 and 1,000,000) by compressing entity numbering, if possible. In some operations the ANSYS^â code performs much slower with large, unnecessary entity numbers and the slow speed will create a corresponding degradation in MC’s checking speed.

• Save your database prior to using MC. This is precautionary only, as every attempt has been made to ensure that your model is not altered. However, MC does make many components, which you may, or may not, want to reside in the database. In addition, repeated passes through the checks may leave components in the database that are no longer applicable to the model. For example, if you run MC requesting the shell normal checks and MC creates 10 shell panels with bad shell normals. You then revise the model and run the shell normals check again and MC finds 4 shell panels with bad normals. Shell panel components for the original panels, 5 through 10, will still exist in the database. The latest HTML report indicates which components are really appropriate for the current database. Obviously, if you had reviewed the results (HTML report and associated components) of the checking, resumed the original database, made the corrections, did another SAVE, and then reran the checks, only the appropriate components would exist in the database.

• Certain checks (net load, mass summary, shell normals, mesh compatibility) are more computationally intensive than others. Request these checks only when essential.

• Load summaries, for models that do not have inertia loads, will run much quicker if a mass summary is not requested.

• Use the “all previous checks” option to streamline repeated checking.

Installing ModelChecker

The installation steps are automated via a self-extracting file (PC), or the use of a tar file, and hence the installation instructions supplied with the files should be followed. The steps listed herein indicate the intent of the install procedures. You should not have to perform most of these steps – only steps 2 and 3 need to be done manually.

To properly install MC for ANSYS, your system administrator should perform the following steps:

1. Copy all macro files (*.mac) to the ANSYS^â APDL directory. Normally this is C:\ Program Files\Ansys Inc\v90\ANSYS\apdl on Windows systems and /ansys_inc/v90/ansys/apdl on UNIX systems, but may have been changed during your initial ANSYS^â installation. If you are unsure as to the location of the APDL directory, you can run ANSYS and enter ‘/inquire, x, APDL’ in the input window. The value of ‘x’ will be shown in the output window and will consist of the correct path to the APDL directory.

2. Copy the license file (caegmc.code) to the ANSYS^â DOCU directory. Normally this is C:\ Program Files\Ansys Inc\v90\ANSYS\docu on Windows systems and /ansys_inc/v90/ansys/docu on UNIX systems. This license file should be obtained from your local reseller/remarketer.

3. Edit the file menulist90.ans located in the ‘UIDL’ subdirectory (normally this is C:\Program Files\Ansys Inc\v90\ANSYS\gui\en-us\UIDL on Windows systems and /ansys_inc/v90/ansys/gui/en-us/uidl on UNIX systems) and add the following line to the end of this file:

For UNIX systems:

/ansys_inc/v90/ansys/gui/en-us/uidl/CAEG.GRN

For Windows systems:

C:\ProgramFiles\Ansys Inc\v90\ANSYS\gui\en-us\UIDL\CAEG.GRN

(Substitute the path to your “UIDL” directory where appropriate.)

4. Copy the granule file (CAEG.GRN) to the UIDL subdirectory.

5. Copy the reasonable values file (reasval.ans) to the DOCU subdirectory

6. Copy the report header file (caegmc.head) to the DOCU subdirectory or, alternatively, your working directory. Edit this file and insert one line of text (a typical entry would be your company name). This “header” will be the first line in the HTML report and is limited to 32 characters. .

7. Copy the resource file, ModelChecker.rc, to the RESOURCE subdirectory - C:\Program Files\Ansys Inc\v90\ANSYS\gui\en-us\resources

8. Copy the script files (xx.eui files) and the index files to the following directories:

modelChecker.eui - C:\Program Files\Ansys Inc\v90\ANSYS\gui\scripts

caegmc_initerr.eui, caegmc_step1.eui, caegmc_step2.eui, caegmc_step3.eui, caegmc_step4.eui, caegmc_step5.eui, caegmc_step6.eui, caegmc_step7.eui, caegmc_step8.eui - C:\Program Files\Ansys Inc\v90\ANSYS\gui\scripts\ModelChecker

tcllndex - there are two different files (with two different sizes) having the same name – place the larger file in the ..\gui\scripts subdirectory and the smaller file in the ..\gui\scripts\ModelChecker subdirectory

9. To have access to the MC users manual online from within ANSYS^â, perform the following:

· Create the MC_HELP directory:

For UNIX systems: /ansys_inc/v90/ansys/docu/en-us/mc_help

For Windows systems: C:\Program Files\Ansys Inc\v90\ANSYS\docu\en-us\mc_help

(Substitute the path to your “DOCU” directory where appropriate.)

· Copy the files from the MC_HELP directory on the supplied file to this directory.

Notes:

1. To view the MC users manual, use an acceptable Web browser (both Internet Explorer and Netscape have been tested).

2. The following files need to be lower case on UNIX:

· reasval.ans

· caegmc.head

· caegmc.code

In general, any files supplied in upper case should be left as upper case (i.e. the macros and the granule file, CAEG.GRN).

Incorrect Summaries from ModelChecker

A user of MC might be quite justified in asking, “Are the summaries in MC always accurate?” The key word here is “always”. Someone can always prove the existence of a software error but no one can prove that any given piece of software is error-free. In our case, MC relies on the following software:

· The ANSYS^â Software

· The utilities that are provided to access information in the ANSYS^â database

· The computation/checks performed by MC

· The coding created to present the results in HTML format

An error in any one of these will cause the HTML report to be inaccurate. MC must be considered a model checking aid, not an infallible expert. MC uses standard and modified versions of ANSYS^â commands to perform the checking and create the HTML report. If such commands generate an ANSYS^â error, MC may, or may not, trap such an error. A simple example of such a problem is a model having very large node and element numbers. Such a model can cause ANSYS^â to “run out of memory” during the operation and hence abort the operation. The corresponding section of the report will be incorrect and some checks are dependent on the results of previous checks. The MC summaries can contain errors, but will, hopefully, still be quite useful for the great majority of models. If an ANSYS^â error occurs during the checking process, the error will be noted in two places:

1. In the General Model Information section of the HTML report, the number of ANSYS^â Errors During Checking is noted. If the number reported is nonzero, review the file caegrpt.err.

2. The file, caegrpt.err, is created while MC performs the model evaluation. This file should be reviewed for errors reported by ANSYS^â by searching for the word “ERROR”. The error message will identify the nature of the problem.

If an error is found that is an MC error, please report it via e-mail (with an example input file or ANSYS^â database) to your local support person. Please avoid sending large (> 1 megabyte) databases via e-mail. Try to create a simple model that shows the same behavior. Please also review the later section, Troubleshooting Models.

Model Checking Options

This section covers the various options that are available for model checking. MC provides comprehensive checking of the solid model, the finite element model, or both. To gain the most benefit from MC, it is best to use it often as the model evolves. We now show the various dialog boxes presented and give a brief discussion of each. The next section, Model Checking Details, provides a detailed discussion of each specific check.

You begin by requesting an evaluation of your ‘in memory’ model from the ANSYS^â Main Menu.

Figure 1: Running MC interactively from the ANSYS Main Menu

A series of Dialog boxes appear that allow you to set the desired level of checking. Each Dialog box has selections that can be requested by “picking” the circular button located next to the selection. After the selections are made you accept them by picking Next. Changes can be made in a prior dialog box by picking the Back button. To leave MC for any reason, pick the CANCEL button in any Dialog box. Detailed help (access to this manual) is available from any Dialog box by picking the HELP button. A brief explanation of each dialog box follows.

Figure 2: Dialog Box #1, Evaluate FE model, the Solid model or both

The Dialog box shown in Figure 2 is self-explanatory. The user should be aware that most of the reported/calculated values are influenced by the currently selected set of entities. If all solid model and finite element entities are not selected, the Dialog box, shown above, gives the user the option to select everything before proceeding. You may evaluate the solid model, finite element model, or both. As before, if solid model entities, or FE entities, are not present in the model, the Dialog box is automatically modified so that the user is alerted that only the solid model, or only the FE model, is available for checking. Based on the choices of this dialog box, MC simply evaluates the currently selected entities of the solid model, the FE model, or both.

The choice, All default chks, bypasses the remaining dialog boxes and performs a basic set of checks based upon MC’s review of the model. Pick Individual allows the user to view the remaining dialog boxes and to make changes/additions reflecting their desired checks. The choice, Previous checks, only appears if a previous check was performed in the user’s current ANSYS^â session and allows the user to skip the remaining dialog boxes and perform the same checks that were performed in the last run.

Figure 3: Dialog Box #2, Solid Model Check Settings

Solid Model checking options include the ability to diagnose and create separate parts based upon topology, detect small geometric features that may increase computational resources, and obtain a complete summary of the model’s volume (or area) and its mass properties. These checks are selected using the menu shown in Figure 3. See Solid Model Checking in the Model Checking Details section for a complete description.

Figure 4: Dialog Box #3, Finite Element Model Check Settings

Finite element model checking is both broad and comprehensive. The checking options are shown in Dialog Box #3 (Figure 4). The checks can create contiguous parts, evaluate the connectivity between the various parts, and thoroughly evaluate the model attributes, loads, boundary conditions, and solution options. The defaults of this dialog box are to perform all applicable checks for the selected set of elements and associated nodes. See Finite Element Model Checking in the Model Checking Details section for a complete description.

Figure 5: Dialog Box #4, Creating components from the identified parts

If either Solid Model or Finite Element model parts creation is requested, MC will save them as named components. In general, use the defaults in Dialog Box #4 (Figure 5). It is very important that the user know whether the model is one integral piece or an assembly and to be able to easily review the parts in an assembly. A very simple naming convention is employed. By default element parts will be named PART1E, PART2E, etc. Volume parts will be named PART1V, PART2V, etc. The user can change the first portion of the part name by altering the default entry in the Generic Name region (see Figure 5).

Figure 6: Dialog Box #5, Load and Mass Summary Options

If either the Net Load or Finite Element Mass summaries have been requested from the Finite Element Model Check Settings dialog box, you may elect to have load and/or mass summaries on the total model only, or of the individual parts and the total model, as shown in Figure 6. If the part-by-part load summary is chosen, an option is available to generate a plot of each part in the load summary section of the HTML report. Each part is shown full size (auto-scaled) unless you set the parameter _caegnofit=1. In addition, each part plot in the load summary section will have a triad in the upper left corner that shows the global directions of X, Y, and Z and hence the load directions. The triad is not showing the location of the global origin.

Figure 7: Dialog Box #6, Plots for the HTML Report

The next Dialog Box allows you to create different plots (Figure 7) and will vary depending on your requests for solid and finite element model checking above. We recommend that you request plots for your HTML report after you have resolved all warnings and errors produced by MC (the default for the first checkbox supports that recommendation). Multiple views of many entity types can quickly create a large number of plots.

Figure 8: Dialog Box #7, Additional Element Plots

The upper region of the Additional Element Plot Choices Dialog box, shown in Figure 8 above, allows the user to color-code the elements based on an element attribute. As a minimum, the user should review non-homogeneous models with the elements color-coded by element type and material number. For assemblies, color-coding the elements by parts allows the user to quickly see which regions of the model will be considered distinct parts. This is a critical plot that should be reviewed in the HTML report.

The lower region of this Dialog box allows the user to decide which, if any, boundary conditions will be shown on element plots. Any selection made here will generate an element plot showing the requested boundary conditions (plots will be made for all views selected in the preceding dialog box).

Finally, having identified the requested checks, MC can be run interactively (immediately) or can be run later in batch mode (Write Batch File), as shown in Figure 9. If the user chooses to run MC later, this option writes the file caegbat.inp that is supplied as the input file when the batch run is executed.

Figure 9: Dialog Box #8, MC Run Options

Batch execution can vary depending on the system that is being used. Follow your batch procedure or use the ANSYS^â launcher. The ANSYS^â launcher, available on both UNIX and Windows systems, contains a Batch option that provides the setup for batch execution. The output file does not contain any meaningful information. The important information is written to the HTML report file, jobname_rpt.html. This file is written to a report directory named jobname_rpt, which is automatically created below the user’s working directory. If you are running on a remote computer, please remember to copy the contents of the report directory to the initiating computer. If plots are requested, plot files and the HTML report will be written to the report directory. In addition, the error file, caegrpt.err, and the output file, caegtmp.out, are copied to the report directory. The output file is primarily used for diagnostic purposes. Users may be asked to forward the output file and the error file if some type of software error occurs. The plot files are accessed from their thumbnail representation in the HTML report. Therefore, all files should be retained.

Notes:

1. When making repeated MC checks (using the same jobname) on a Windows NT platform, MC will not be able to create a new HTML report in the jobname_rpt subdirectory, if that subdirectory is “open” in Windows Explorer. The HTML report will be created and is still usable but is not in the correct directory. If the subdirectory is “open” (by mistake), the HTML report and plots will be placed in the working directory.

2. The jobname portion of the HTML report filename and directory name will be truncated to the first 23 characters if the actual jobname has a longer name.

Model Checking Details

In this section we cover the details of the various checking options, discuss problems that routinely occur in finite element modeling, and describe the HTML report that is produced. We begin with Solid Model Checking and then cover Finite Element Model Checking.

Solid Model Checking

Solid model parts -

MC can evaluate the solid model as well as retrieve the quantities of all solid model entities; volumes, areas, lines and keypoints. When the option is set to “Make solid model parts”, MC checks the connectivity (topology) of the selected solid model entities. Volumes that share common areas will act as an integral unit, i.e., one part, when meshed and analyzed. Similarly, areas that share common lines and lines that share common keypoints behave as integral units. If you bring 40 volumes into ANSYS^â from a CAD system, or build 40 volumes in ANSYS^â, you need to know whether this model will behave as one integral unit or an assembly of two or more parts (perhaps 40 parts). The solid model parts are saved as named components. The default naming convention for these components is as follows: PART#V for volumes, PART#A for areas, and PART#L for lines, where # is the assigned component number.

Small entity checks -

The small entity check phase will determine the magnitude of the largest and smallest volumes, areas and lines, as well as the associated entity numbers. The goal of the small entity check is to identify small features: short lines, small areas and volumes.

Figure 10: Examples of Small Geometric Features

These features may be relevant to the analysis, but quite often the solid model has small features that are present due to loose geometric tolerances, or construction techniques, employed in the CAD system. Small entities should be reviewed for their appropriateness before meshing the model. This can save both time and effort because small entities usually increase the number of elements in the model and make meshing considerably more difficult. In addition, the solution time step for an explicit transient dynamic analysis is governed by the wavelength of the material, which is automatically calculated using the smallest element’s length. Small features that are present in the geometry often lead to small elements that, in turn, lead to a very small solution time step and very long run times. Small features are shown in Figure 10 and may require cleanup in the originating CAD product or by using a CAD cleanup software tool.

Two array parameters are stored if the small entity check is requested: CAEGLLI_ (lines) and CAEGAAR_ (areas). They contain the line #/area # and line length/area magnitude for the selected lines/areas in ascending order of entity magnitude. The information contained in these arrays can be listed using the ANSYS^â command *STATUS. Additionally, two macro commands (the macros are automatically installed during ModelChecker installation) can be used to select (or add to the current selected set) a sequence of lines or areas as stored in these small entity check arrays. For example, CAEGLUTY.MAC (lines) (CAEGAUTY.MAC the utility for areas is used in a similar manner) can be used as follows:

CAEGLUTY,3,18,1 - selects lines in array positions 3 through 18 from the entire model; the 1 in the third field indicates a selection from the entire model.

CAEGLUTY,3,18,2 – lines in array positions 3 through 18 are added to the currently selected lines; the 2 in the third field indicated that an add to the selected set is to be done.

CAEGLUTY,3,18,3 – lines in array positions 3 through 18 are selected from the currently selected lines; the 3 in the third field indicated that a select from the currently selected set is to be done.

As a rule of thumb, Small entity checking should always be done before meshing to:

· Prevent many unnecessary elements from being generated

· Reduce the number of distorted elements

· Maintain a manageable finite element model size

Small Angles

Small angles between lines usually result in poorly shaped elements, very dense meshes, or may cause meshing failures. If the small angle check is selected, selected keypoints that have small angles (user defined) between their lines are grouped into the component CAEGKANG. The HTML report includes the number of keypoints having lines with small angles and the smallest and largest angles found during the check of the selected keypoints.

Further, if such keypoints are found during the small angle check, an array parameter CAEGKAN_ is stored and contains the angle and line numbers. The information contained in CAEGKAN_ can be listed using the ANSYS^â command *STATUS.

Contents of array parameter CAEGKAN_:

Column 1 – keypoint number

Column 2 – angle between the lines (degrees)

Column 3 - first line number

Column 4 – second line number

We check the angle between every pair of lines that connect to the selected keypoints. Some of these lines may not be in the same area and hence a small angle is not a consideration unless you have/make a volume that contains these lines.

Volume/Mass summary -

Finally, the Volume/Mass summary request will provide the total volume for the entire model and its center of mass location with respect to the global Cartesian origin. As usual, the volume and mass summary is based on the selected set.

Note: The mass summary is computed using the densities associated with the higher-level geometric entities. If none of the associated densities are defined, then a unit density is used. The mass and center of mass values are given for the set of selected volumes unless there are no selected volumes. In this case, they are based on the selected areas using the associated real constant thickness if the associated element type supports thickness. If not, the area mass is based on a “unit thickness”. Furthermore, the total area of the selected set of areas is listed instead of the total volume when there are no volumes in the selected set.

HTML Report Information -

The following Solid model information is included in the HTML report.

Solid Model Entity Summary -

	Largest Number	Number Defined	Number Selected
Keypoints
Lines
Areas
Volumes

Solid Model Diagnostic Information -

Parts Summary: Number of Volume, Area, and Line Parts

Small/Large Entity Summary:

Largest Volume/Volume # Smallest Volume/Volume #

Largest Area /Area # Smallest Area/Area #

Largest Line/Line # Smallest Line/Line #

Small Angle Summary:

# of Keypoints containing lines with small angles

Smallest/Largest angle between checked lines

Volume/Mass Summary (based on selected entities):

Total Volume or Area

Total Mass

Location of Center of Mass

See Sample HTML Report

Finite Element Model Checking

The element types used in the model are at the core of any finite element analysis. They determine the dimensionality (2D or 3D), the allowed response given the applied loads (the degrees of freedom), and the overall behavior (linear or nonlinear). One of the tasks performed by MC is to determine which element types are used (have associated elements) and whether the element types are compatible with each other, the type of loading, nonlinear behavior, etc.

Let’s examine each of the finite element model checks.

Element Parts –

An element part is a group of connected elements, which, during analysis, will act as one integral piece (part). Even if elements only connect at one node, such elements are deemed to be in the same part, i.e., adjacent (2-D and 3-D) elements do not have to share an entire face to be in the same part. Obviously, in most instances, elements should share entire faces, rather than a node, to ensure displacement compatibility. In a later menu (see: Figure 5) the user will have the option to ignore, or include, each of the following, in determining how many element parts are in the model:

· Coupling equations

· Constraint equations

· 1-D elements (spars, beams, gaps, etc.)

If included, coupling and constraint equations are treated as elements with nodes (from the coupling and constraint equations) when determining parts. Contact elements (library names CONTAxxx and TARGExxx) are always ignored when determining parts. The HTML report will list the number of element parts and the basis for determining parts (the user settings for including/ignoring coupling, constraint equations and 1-D elements if such quantities/entities exist in the model). The number of finite element parts is even more important than the number of solid model parts (discussed earlier). The number of element parts dictates whether the analysis model is viewed by ANSYS^â as an integral unit or an assembly of individual parts. Furthermore, if it is an assembly of separate parts, it is useful to know the number of parts and the mass and loading contributions of each part.

Element Checks –

All elements in the model are checked for completeness, acceptable shape and compatibility with each other. The HTML report summarizes the following:

· # of Isolated elements (not connected to other elements)

· # of Unused Element Types, Materials, and Real Constants

The maximum number of unused real and material sets listed in the HTML report can be limited by defining the values of the parameters _caegrl and _caegml, respectively, before running MC.

· # of Needed (but undefined) Materials and Real Constants

· # of Elements with Mesh shape warnings and errors

· # of Specialty elements in the model such as:

Superelements

Contact/Target elements

Pretension elements

Gasket elements

p-elements

Mesh 200 elements

Surface Effect elements

Shell elements

Axisymmetric elements

Harmonic elements

Composite elements

Lumped Mass elements

1-D elements

Isolated elements are usually causes of concern since, in the absence of coupling or constraint equations, such elements behave independently, often resulting in undesirable rigid body motion. These elements are defined as component CAEG1E.

Note: If the user has chosen the defaults for creating finite element parts (see Figure 5), 1-D elements are excluded and won’t be checked for isolation.

Unused element types, materials and real constants are of no real concern unless they were intended to be used in the model. One note of caution, however: element types that are unused affect what ANSYS^â considers to be the active DOF in the model. For instance, if you build a model with SOLID45 elements (8-noded bricks having UX, UY, and UZ DOF) and have an unused (no elements) SHELL63 element type, ANSYS^â considers that the valid DOF at any node are UX, UY, UZ, ROTX, ROTY, and ROTZ (the DOF of SHELL63). The user will be allowed to apply moments to the SOLID45 element nodes. However, these loads will be ignored during the analysis since the SOLID45 element nodes do not have rotational DOF. No warning messages will be given in the analysis. In the HTML report, we list the real active DOF in the model based on the elements, rather than the element types, defined.

Needed (but undefined) materials and real constants are quantities that must be defined before the analysis can be run.

NOTE: ModelChecker does not currently check for needed but undefined, or defined but unused SECTION Properties, this capability is will be added in a future release.

Elements with shape warnings are grouped as component CAEGEWRN and those with errors are grouped as component CAEGEERR. Obviously, the elements with errors must be fixed before the analysis can be run. The elements with warnings should be reviewed to see whether the warning, and the elements location within the model, is such that the impact might be significant. The warning and error criteria, employed by MC, are based on the current shape checking warning and error limits (see the ANSYS^â Theory Reference, Section 13.7 and the ANSYS^â command SHPP). MC will not permit the execution of the Net Load and Mass Summary checks if shape errors are present, regardless if shape error checking has been deactivated (SHPP,WARN or SHPP,OFF). The HTML report gives a very concise summary indicating the number of elements that fall into each category and the worst characteristics of such elements, e.g., the largest aspect ratio, the largest interior angle, etc.

The list of specialty elements is useful for verifying the existence of element types that can significantly affect the behavior of the model. For example, a user may discover that the model contains axisymmetric elements whereas plane strain elements were intended. If either axisymmetric and/or harmonic specialty elements are present and selected prior to checking, MC checks the following:

Axisymmetric elements – A mixture of axisymmetric and other elements will generate a warning. The mixture of elements may be perfectly acceptable, however, extreme care should be taken when mixing other element types with axisymmetric element types. Inertia loads are checked to ensure that loads are consistent with axisymmetric deformation. Improper loads will generate a warning and improper inertia loads are listed in the HTML report.

Axisymmetric-Harmonic elements - A mixture of axisymmetric-harmonic and other elements will generate a warning. The mixture of elements may be perfectly acceptable, however, extreme care should be taken when mixing other element types with harmonic element types. Additionally, if the analysis is nonlinear, the existence of harmonic elements (which are linear) is questionable and will generate a warning.

Shell Normal Checks –

When shell normal checking is requested, MC uses a modified form of the ANSYS^â ENORM capability to look for adjacent elements with reversed (inconsistent) normals. The software starts with the lowest numbered, selected shell element and finds all adjacent shell elements until the edge of the model is reached or more than two elements (in the entire model, not just the selected set) share a lateral (side) face. Using this method, shell elements are grouped into panels. Elements in each panel are then checked for consistency. If one or more of the shell elements in any panel have inconsistent normals the panel elements are defined as a component CAEGSXXX. The HTML report indicates the number of panels and their respective component names.

Note: There is a limit on the number of shell panel components created by MC. The value can be increased from 300 (default) to an upper bound limit of 4000 by creating the user-defined variable, _caegsp. See Appendix B for more details on this and other user-defined variables.

The problem elements in each panel can be easily corrected by:

1. Selecting the panel component

2. Applying the ANSYS^â ENORM command or the ENSYM command

Note: MC does not perform any corrective action.

This method of checking allows MC to handle branched shell models (see Figure 11), where panels can be checked for consistency, but no unique normal exists for the entire model. However, a model that has overlaid shell elements (two or more elements using the same nodal connectivity) causes this logic to fail since every element will be considered a panel with one element. Therefore, the checks will take a long time and no reverse normals will be detected in such regions since every panel will only have one element. ANSYS^â Powergraphics will display shell elements with reversed normals by applying different colors. However, visual inspection can be very labor-intensive and error prone on complex models.

Figure 11: Shell normal orientation displayed using ANSYS Powergraphics

Shell surface normal orientation is determined by the order of the connected nodes, either clockwise or counter-clockwise. The orientation controls the direction of applied surface pressures and the definition of the “top” and “bottom” surfaces of the shell, where bending stresses are computed.

Two problems can occur when there are adjacent shell elements having reversed normal orientation:

1. Average nodal stress result listings and plots for adjacent elements with reversed normal orientation are meaningless except at the shell middle surface, unless ANSYS^â Powergraphics is active. ANSYS^â Powergraphics detects shell element orientation and averages the stress results, correctly, based upon the orientation of adjacent elements.

2. Since pressure loads are interpreted in the element coordinate system, the total load from applied pressures is usually misleading and incorrect when some element normals are reversed (see Figure 12). This can be remedied by applying positive pressure to some elements and negative pressure to others, but it is usually preferred to simply reorient the element normal to be consistent with its neighbors using the procedure described above.

Figure 12: Inconsistent shell element orientations – applied pressure

Nodal Checks –

MC performs four different nodal checks. These include checks for unused nodes, degree of freedom mismatches, applied nodal loads/displacements without corresponding degrees of freedom, and applied load/specified displacement conflicts. The simplest nodal check is to look for unused nodes. Unused nodes are more of a nuisance than a source of error. However, leaving such nodes in a model is considered bad practice since users will be allowed to select these nodes, they appear in nodal plots, and, more importantly, loads applied to these nodes will be ignored during the solution. Unused nodes are defined as component CAEGUN.

A very important check on non-homogeneous models having multiple element types is a check for nodes shared by elements having different degree of freedom (DOF) sets or a so-called DOF mismatch. DOF mismatches should always be reviewed. In most cases, ANSYS^â allows elements of any type to connect at common nodes, regardless of whether the connection makes any physical sense. Attempting a solution with a model containing such mismatches could result in a solution that will (a) not run, (b) yield wrong results by eliminating DOFs, or (c) run normally, but yield questionable results. Corresponding solution messages/characteristics are:

a) Negative Main diagonal – unsupported or restrained DOF

b) Negative Pivot – removal of DOF completely

c) Normal Solution – results should be checked very carefully since elements only transfer loads, at most, in the directions of their DOF.

Figure 13: Indeterminate problem created by DOF Mismatch

In the model shown in Figure 13, the beam element cannot transfer moment (load corresponding to the ROTZ DOF) at the connection with the 2-D solids and hence the model is unstable. Under shear or moment loading, the cantilever section deflection is indeterminate (using small deflection theory). Constraint equations or edge beams need to be added to this model to restore stability.

Two components are saved that contain DOF mismatch information:

CAEGMIS – nodes with DOF mismatch

CAEGMISN – nodes with mismatch and no corresponding constraint equations

Finally, the last set of nodal checks is to search for imposed displacements and applied forces/moments with no corresponding DOF or conflicts between displacements and forces. MC determines the real active DOF in the model based on the element types (with selected elements) used in the model at any given node. Any displacement/load (that is applied to a node) that is inconsistent with the active DOF in the model is considered to be inappropriate and generates a warning. In addition, if applied forces/moments at a node conflict with the imposed displacements at the same node (e.g., user specifies UX and FX at the same node), a warning is generated. Nodes having such boundary conditions are grouped into components and create a warning in the HTML report. The following component names are used:

CAEGUDIS - nodes with imposed displacements with no corresponding DOF

CAEGUFOR - nodes with applied forces/moments with no corresponding DOF

CAEGUFC - nodes with imposed displacements and applied forces/moments conflicts.

This check is very rigorous and accurate; however, it does have one limitation. MC does not account for DOF supplied by Superelements (this is noted in the HTML report).

Mesh Compatibility Checks –

To maintain displacement compatibility (or continuity) at inter-element boundaries, adjacent elements must share all of the nodes on a given edge or face of an element. Discontinuities often result when adjacent elements improperly share nodes (corner vs. mid-side), the elements are a mixture of linear and quadratic elements (see Figure 14), or the underlying, adjacent solid model entities were not sharing common geometric entities at the interface and hence the mesh was not required to “line up” during the meshing operation (See Figure 15). MC will flag adjacency mismatches for planar, solid and shell elements. The current version of MC does not flag discontinuities that result from adjacent linear and quadratic elements (see bottom elements in Figure 14). MC for ANSYS^â 9.0 will flag such discontinuities . Shell elements cannot accurately predict stresses at shell branches/intersections and hence the stress results at such intersections (regardless of node sharing by adjacent elements) should not be considered valid, and require further analysis, such as submodeling with solid elements, to obtain a more accurate result. The mesh compatibility check for shell elements will sometimes flag elements at T-junctions as having mesh compatibility problems. This is an inherent limit in the MCHECK compatibilities that we will attempt to improve at the next release. To bypass the mesh compatibility checks for shell elements, set the parameter, _caegmk= -3, before starting MC.

Figure 14: Incompatible 2D Mesh examples

Figure 15: Sample non-aligning mesh of two non-sharing regions

The mesh compatibility checks for proper adjacency and further utilizes a modified form of the ANSYS^â MCHECK command to detect inverted, hourglass-shaped, or negative volume elements as follows:

· Normal check – for area elements sharing a common edge, ensure that the ordering of the nodes (i, j, k, etc.) is consistent with their relative normals.

· Volume check – for volume elements that share a common face, ensure that the integrated volume of each element is consistent.

· Closed surface check – checks for unintended cracks by verifying that element exterior faces form simply-connected closed surfaces.

· Check for holes in the mesh – checks for voids or accidentally omitted elements.

Elements that produce Mesh compatibility warnings are grouped in the component CAEGMESH and the count is reported in the HTML report. If an error is detected during MCHECK (e.g., ANSYS^â runs out of memory), the error message is placed in the Mesh Compatibility section of the HTML report.

In addition, the memory required for some operations is dependent on the largest node and element numbers. The memory required appears to be (at least) 200 times the largest element number in the model. For models with very large node and element numbers, set the ANSYS^â workspace (- m) to as large a value as possible and, after checking is completed, check the General Model Information section of the HTML report. If the Number of ANSYS Errors During Checking is greater than zero, please review the error file (caegrpt.err) and search for the word ERROR to see if MCHECK caused the program to “run out of memory”.

Coupling Equation Checks –

Coupling equations most often ‘join’ coincident nodes between mating parts. Coupling is often used to enforce symmetry, to introduce a frictionless surface, and to define pin joints. The coincident nodes are joined to act as one in any or all degree of freedom directions. Sources of error come about when nodes that are not coincident are coupled. This can introduce artificial moments resulting in incorrect results, as shown in Figure 16. Note the “missing moment” is equal to the vertical shear load times the horizontal separation distance. Non-coincident coupled nodes are flagged (create a warning), counted and grouped as component CAEGNCCP. Nodes are considered non-coincident if the separation distance exceeds a given tolerance. The default tolerance is 1.0E-04 (model length units) and can be over-ridden by defining the value of the parameter, _caegcpt, to be the desired tolerance before running MC.

Additionally, coupled nodes having dissimilar nodal coordinate systems are also flagged, counted and reported as component CAEGNPCP. Coupling forces two or more nodes to move the same amount in a given nodal DOF direction, e.g., UX. In most cases, the user wants the nodal coordinate system to be the same for all nodes in a given coupling set. For instance, if one was modeling a frictionless interface between two inclined faces in an assembly, an inexpensive modeling approach would be to ensure that the node pattern on both parts “line up”, and then couple the corresponding nodes in the direction normal to the interface. This requires the user to rotate (see ANSYS^â NROTAT command) the nodal coordinate system for both sets of nodes so that one DOF direction is normal to the surface. If both sets have not been rotated, the MC software will flag the model with a warning and put the nodes from each coupling set in component CAEGNPCP. Nodal directions are considered to be non-parallel if any of the nodal angles, for any node in the coupling set, differ by a given tolerance. The default tolerance is 1.0E-01 (degrees) and can be over-ridden by defining the value of the parameter, _caegcpa, to be the desired tolerance before running MC.

In some instances, non-coincident and non-parallel nodal coordinate systems are needed from a modeling viewpoint. A simple example would be a model that is rotationally periodic (cyclically symmetric). In this case, we model the smallest repeatable segment and impose the condition that, in a cylindrical coordinate system, nodal displacements, at the corresponding nodes on the left and right faces of the segment, must be the same via coupling equations. The coupling checks should not be used for cyclic symmetry models or the cyclic symmetry regions should be unselected before requesting a check. To avoid performing the coupling checks on the cyclic symmetry faces, before running MC, define the nodes on the cyclic symmetry faces as component caegnocp. Nodes in component caegnocp will not be subjected to the coupling checks regardless of which nodes are selected when MC is invoked.

The coupling checks can be quite CPU – intensive on large models. Only coupling equations having all nodes selected are checked for non-coincidence or non-parallel directions. To avoid user frustration when coupling checks are inadvertently requested on a cyclic symmetry model or any large model with a large number of coupling warnings, MC will automatically stop further coupling checks when the number of coupling warnings due to non-coincident and/or non-parallel nodal systems exceeds 100. This limit can be over-ridden by setting the value of the parameter, _caegcpl, to the desired limit before running MC.

The program also checks to see if large deformation effects (NLGEOM) are turned on. If so, the model is given a warning since the coupling equations are based on nodal positions and nodal displacement directions of the un-deformed model and hence may be incorrect during large deformation.

Figure 16: Coupled Non-coincident nodes

Constraint Equation Checks –

Constraint equations are used to connect dissimilar meshes (see Figure 17), define rigid regions, model interference fits, and tie together dissimilar DOF elements. Improperly defined constraint equations can artificially stiffen a model and may also introduce a local artificial high stress or ‘stress riser’. The constraint equations are evaluated for correctness by subjecting them to a displacement field equivalent to a quasi-free thermal expansion loading. The assumed displacement field is simply UX=X, UY=Y, UZ=Z, ROTX=ROTY=ROTZ=0. The constraint equation is rewritten as ( expression ) = 0. The expression is evaluated by inserting the known values of the nodal displacements (obtained by inserting the known nodal coordinates into the assumed displacement field). The evaluated expression (residual) is checked against the allowable value, by default, 1.0E-06. Any constraint equation generating a larger residual value generates a warning in MC. The default allowable value is somewhat arbitrary and the user can override this value by setting the parameter, _caegrsd, before running MC. Correctly defined constraint equations do not introduce significant artificial loads. Any constraint equation that cannot be satisfied, when assigned displacements corresponding to a uniform thermal expansion, has its number listed in the HTML report and its associated nodes are grouped into the component CAEGCEN. Additionally, constraint equations are also based on small deflection theory and, hence are flagged if the solution allows large deflections (NLGEOM,ON).

Note: The checking may flag constraint equations that are perfectly fine for use. For example, a rigid region may be defined using the ANSYS^â command CERIGID. The resulting constraint equations will generate a warning message because the region cannot expand when subjected to the displacement field consistent with a uniform temperature rise. If your constraint equations are of this type, then do not request constraint equation checking, but also recognize that thermal loads may introduce significant stress in regions adjacent to the rigid region.

Figure 17: Connecting dissimilar meshes using constraint equations

To avoid HTML reports having long listings of constraint equation numbers generating warnings, the number of constraint equations listed in the HTML report is arbitrarily limited to 100. This default can be over-ridden by setting the parameter, _caegcel, to the desired limit before running MC.

Temperature Checks –

The model is checked for temperature completeness/consistency, appropriate material properties, and reference temperatures. Nodes and elements are checked to determine if all entities or only a portion of these entities possess applied temperatures. For instance, if only some of the nodes have applied temperatures then the remainder will default to TUNIF, which might be incorrect, and hence result in significant local differences in thermal strain. It is very important to identify such “gaps” in applied temperature because they can result in considerable thermal stress. These checks will also identify potential conflicts in applied temperature. For example, if temperatures are applied to both nodes and elements, the element temperatures will take precedence and be used in the solution. There are ten possible situations that MC can identify:

1) All nodes have applied nodal temperatures and all elements have defined element temperatures.

2) All nodes have applied nodal temperatures and some elements have element temperatures.

3) All nodes have applied nodal temperatures and no elements have element temperatures.

4) Some nodes have applied nodal temperatures and all elements have element temperatures.

5) Some nodes have applied nodal temperatures and some elements have element temperatures.

6) Some nodes have applied nodal temperatures and no elements have element temperatures.

7) No nodes have applied nodal temperatures and all elements have element temperatures.

8) No nodes have applied nodal temperatures and some elements have element temperatures.

9) No nodes have applied nodal temperatures and no elements have element temperatures.

10) No elements supporting element temperature loading (using the ANSYS^â BFE command) are selected.

Any temperature distribution, except as described by 3 and 7 above, will create a warning in the HTML report if the temperature check is requested.

MC will perform the following checks to determine the nature of the temperature field:

· Are Element temperatures applied to all/part/or none of the elements? If the model has temperatures applied to some elements, the remaining elements, without temperatures, are grouped into the component CAEGELMT.

· Are Nodal temperatures applied to all/part/or none of the nodes? If the model has temperatures applied to some nodes, the remaining nodes, without temperatures, are grouped into the component CAEGNOMT.

· Does the model contain defined or undefined uniform (TUNIF) and reference (TREF or REFT material properties) temperatures? Differences in REFT and TREF values are also examined.

· How many materials are used in the model and what is the number of defined coefficients of thermal expansion, ALPHA?

· Are any temperature-dependent material properties defined?

Models with no ALP(x, y or z) create a warning, as do models without any temperature-dependent material properties. An incomplete temperature specification, TREF, REFT, or ALPHA could yield inappropriate thermal expansion effects and/or improper evaluation of temperature dependent material properties.

Check for Reasonable Values –

Material properties, loads and temperatures can be examined for reasonable values to alert the user to possible unit problems and/or typographical errors and hence eliminate unnecessary solutions that may yield incorrect or nonsensical results. The ANSYS^â program assumes that all dimensions, material properties and applied loads are based on a consistent set of units. However, it is up to the user to verify the values, which include material properties, dimensions, and loads. There can be a wide range of values depending on the unit system that is applied. For example, if you are analyzing a MEMS (micro-electro-mechanical) device, the length units may be in micrometers (mm or 10^-6 meters). Some comparable dimensions are:

Structural Value	SI Unit	Dimension	m SI Unit	Conversion Factor
Length	Meter, m	m	mm	10^6
Force	Newton, N	(kg)(m)/(s)^2	mN	10^6
Time	Seconds, s	s	s	1.0
Mass	Kilograms, kg	kg	kg	1.0
Pressure	Pascals, Pa	(kg)/(m)(s)^2	MPa	10^-6
Velocity	Meters/second	m/s	mm/s	10^6
Acceleration	m/(s)^2	m/(s)^2	mm/(s)^2	10^6
Density	Kg/(m)^3	Kg/(m)^3	Kg/(mm)^3	10^-18
Young’s Modulus	Pa	(kg)/(m)(s)^2	MPa	10^-6

Some loadings should also be subjected to these checks. For instance, an organization may know that their parts/systems can never be subjected to temperatures exceeding 2500 degrees. The reasonable value temperature maximum should be set to this value to ensure that temperature boundary conditions that exceed this limit are subjected to more scrutiny. The high temperature value may be employed for a legitimate modeling purpose, but the user/contractor/manager should be alerted to such temperature loading. Angular speed (OMEGA) is another simple load whose minimum and maximum values are commonly known throughout an organization. A new user, or a user accustomed to another FE program, might input a speed that is dimensionally incorrect and hence be outside of the reasonable value range.

When the reasonable value check is requested MC looks for the file reasval.ans. We strongly recommend that a modified version of this file be made available to each user or that a universal version be made applicable to all users in the organization. To accomplish this, the ANSYS^â software uses a search hierarchy for all files using the .ans extension. The search is done in the following order:

1) Current Directory

2) Home Directory

3) Documentation Directory - \Program Files\Ansys Inc\v90\Ansys\docu

Therefore, an organization can place a standard version of the file reasval.ans in the documentation directory and each user can place a customized version in either their home directory or their current (working) directory. The standard MC installation procedure puts a sample copy of reasval.ans in the ANSYS^â Documentation directory; the checking values supplied in this file must be changed before use. The default checking values have a very large range and hence are of little value. The View File selection will allow review of the current settings – modifications can be made by editing the file independently.

The following items are checked for reasonable values:

Material Properties (evaluated at the reference temperature (TREF)):

EX, EY, EZ, GXY, GXZ, GYZ, NUXY, NUYZ, NUXZ, PRXY, PRYZ, PRXZ, ALPX, ALPY, ALPZ, REFT, MU, DAMP, DENS

Loads:

ACEL-X, -Y, -Z

OMEGA-X, -Y, -Z

DOMEGA-X, -Y, -Z

Temperatures:

TUNIF, TREF, Nodal temperature values, Element temperature values

A sample version of reasval.ans is provided with the MC software and the contents of this file are shown in Appendix C. If the file does not exist or does not have the correct name, MC will allow you to browse your system for the location of the file.

Figure 18: Locating the reasonable value range file

FEM Mass Summary –

The finite element model is intended to correctly represent the behavior of the actual structure. This behavior is characterized by the mass and stiffness of the structure. The intent of the FEM mass summary is to verify the total mass of the structure and/or the mass of the individual parts in an assembly. If the mass is inaccurate, it is highly likely that the stiffness is inaccurate. In many cases, the user knows the weights of the individual parts in an assembly and a part-by-part check of the masses yields more confidence that the geometry was represented accurately and the proper density has been assigned to each part.

The individual element (selected elements only) contributions are summed to obtain the mass and center of mass of the model. The center of mass is given with respect to the origin of the global Cartesian coordinate system. The mass summary requires that the element mass matrices be formed and, hence any feature of the model that would prohibit formulation, e.g., an undefined but needed real constant, will cause the mass summary to be by-passed. The mass summary request also requires the ANSYS^â program to make the file caegrpt.emat, and sometimes caegrpt.esav. This file(s) is subsequently deleted, but may require significant disk space while the model is being checked.

The mass summary and center of mass can be requested for the entire model or, part-by-part, as well as the entire model.

The HTML report also indicates how many, if any, of the elements do not have density defined.

Notes:

1. The FEM mass summary does not presently support p-elements, explicit elements, and harmonic elements. If such elements are present in the model, the mass and net load options are automatically eliminated from the Dialog box choices. To evaluate such models, temporarily change their element types to a corresponding ANSYS^â standard structural element type and perform the check. This “trick” can also be used with thermal or electromagnetic models.

2. The harmonic elements that are affected are PLANE25, SHELL61, FLUID81, and PLANE83. These elements can be temporarily converted to the axisymmetric versions of PLANE42, SHELL51, FLUID79 and PLANE82, respectively. If the model consists of a mixture of 2-D and 3-D elements, the values given in the mass summary, other than in the x and y- directions, may be incorrect. This is an inherent limitation in the ANSYS^â mass calculation.

3. If MASS21 elements are present and the mass values are different in the x-, y- and z-directions, the mass contribution of these elements is inaccurate due to an approximation used in the internal ANSYS^â mass summary calculation (mass = (mx + my + mz)/3).

4. The FEM Mass summary is a compute intensive calculation that is done using the ANSYS^â solution processor (using a modified version of the ANSYS^â PSOLVE feature). The PSOLVE feature is only available for the products ANSYS^â/Multiphysics, Mechanical and Structural. The FEM Mass summary check is not available for the products ANSYS^â /Professional or PrepPost.

5. If MC hangs during the FEM Mass summary calculation or the HTML report indicates there has been a PSOLVE failure, please refer to the section Troubleshooting Models for possible remedies.

Net Load Summary –

The purpose of a finite element analysis is to mathematically calculate the response of the structure due to the applied loads. Before solving for the response, it is very important to verify that loads are correct in both magnitude and orientation. This check can be, and should be, performed on all of the load cases that are to be solved. Remember, the software is operating on the “in-memory” model and, if you are using load step files, you should bring each set of boundary conditions into the database and run MC on the new in-memory model.

The net applied load check will identify the magnitude, direction, and type of applied loading and lists the global Cartesian components for the selected model subset, each individual part, or both. The load summaries take into account all loadings - solid model and finite element loads. To account for the applied solid model loads, the solid model loads on the selected solid model entities are automatically transferred to the selected elements and associated nodes.

The load summary performs an element-by-element load calculation and gives a force and moment summation about the global Cartesian coordinate system origin. As in the mass summary, if inertia loads are present, the element mass matrices will be formed. Missing materials, real constant sets, etc. will cause this calculation to be by-passed as well.

Reported values include the total applied loads as well as the individual contributions from inertia loads, surface loads, and nodal loads. Body loads from temperatures are not reported since such loads should automatically balance each other and produce no net load.

1-D Elements

If a model includes 1-D elements (with loads applied to the 1-D elements) and a part-by-part load summary is requested where parts are to be made excluding 1-D elements, the net load totals for the entire model may not be equal to the sum of the part totals and may not be correct. The example in Figure 19 is used to explain how MC accounts for loads applied to nodes that are shared between 1-D elements and other elements and loads that are solely applied to the 1-D elements. To avoid double counting of loads, MC removes all contributions from the nodal load totals created by 1-D elements. This means that the 300 lb. shared load is added once (from the 2-D elements) in calculating the entire model total load. However, the 500 lb. load is excluded from the net load summary for the entire model. This approach is not perfect, but in most cases intermediate loads applied to 1-D elements are rare. In addition, the part-by-part summary will include, as the last part, the loads on all of the 1-D elements and the nodal loads will be correct on this part.

Figure 19: 1-D elements with applied loads

This problem only arises when a part-by-part summary is requested and the user has chosen to exclude 1-D elements in making parts. If the user requests a load summary for the entire model (total only), or includes 1-D elements in making parts, the net loads will be correct.

Notes:

1. The net load summary does not presently support p-elements, explicit elements, and harmonic elements. If such elements are present in the model, the mass and net load options are automatically eliminated from the Dialog box. To evaluate such models, temporarily change their element types to a corresponding ANSYS^â standard structural element type and perform the check. This “trick” can also be used with thermal or electromagnetic models. The harmonic elements that are affected are PLANE25, SHELL61, FLUID81, and PLANE83. These elements can be temporarily converted to the axisymmetric versions of PLANE42, SHELL51, FLUID79 and PLANE82, respectively. The interpreted applied loading that is computed for these axisymmetric elements is based on true axisymmetric behavior.

2. The Net Load summary is a compute intensive calculation that is done using the ANSYS^â solution processor (using a modified version of the ANSYS^â PSOLVE feature). The PSOLVE feature is only available for the products ANSYS^â/Multiphysics, Mechanical and Structural. The Net Load summary check is not available for the products ANSYS^â /Professional or PrepPost.

3. If MC hangs during the Net Load summary calculation or the HTML report indicates there has been a PSOLVE failure, please refer to the section Troubleshooting Models for possible remedies.

Simple Rigid Body Motion Check –

The selected set of elements is examined to determine if the constraints are such that rigid body motion is prevented. Figure 20 shows a 3-D solid model with five (5) constraints; rigid body rotation about one axis is not restrained. With the proper additional restraint, rigid body motion is prevented. By default, MC considers the finite element model to be one integral part when performing the simple rigid body motion check. The current check ignores the effects of coupling and constraint equations in restricting rigid body motion. In most cases these equations provide enough additional restraint to eliminate rigid body motion. We hope to include such effects in a future release and be more rigorous in this check - a typical developer’s promise.

The software uses the active DOF for the entire model to try to determine what types of constraints are needed to prevent rigid body motion. This check may uncover basic problems in the overall model, but will not uncover individual stability problems in an assembly. Individual parts should be constrained or should be connected to other parts by either contact or coupling/constraint equations. Please be aware that this check is a more heuristic check, is not rigorous, and may not always be reliable.

The checks are based on examining the active DOF in the model, “divining” the intent of the user, and seeing if the required constraints are in place. For unusual combinations of DOF, the intent may be unclear and hence MC cannot estimate either of the following:

· Number of constraints required to restrain rigid body motion

· Additional constraints needed to prevent rigid body motion

In such cases, the Simple Rigid Body Motion Check section of the HTML report will list the word “unknown” instead of giving numbers for each of the above.

The user can evaluate individual parts for rigid body motion as follows:

1. Run MC to determine finite element parts

2. Save the database to a named file

3. Select any given part and request a rigid body motion check

4. Restore the database of step 2, repeat step 3 for the next part, etc.

Figure 20: Constraining to prevent free rigid body motion

HTML Report Information –

The HTML report contains a complete summary of the Solid and Finite Element models and also includes a diagnostic report for each. MC provides some very unique information in the HTML report that could save many hours of model review and debugging. The unique information, outlined below, is model information that would be very difficult, or impossible, to obtain (in a concise format) using standard ANSYS^â commands. This information is quite valuable regardless of whether the model checking capabilities uncover any questionable aspects of the model.

Unique model features that are reported, beyond standard listings such as the ANSYS^â global status, include:

Finite Element Model Entity Summary

· Used Element Types (with elements) and # of elements for each type

· Used Material Numbers, # of elements of each material number, and basic properties, also indicates if nonlinear properties are defined for each used material

Finite Element Boundary Condition Counts

· # of imposed displacements in each direction for the selected nodes

· # of imposed forces/moments in each direction for the selected nodes

· # of imposed nodal temperatures for the selected nodes

· # of imposed element temperatures for the selected elements

· # of selected elements subjected to pressure loadings

Basic Finite Element Solution Information

· ANSYS^â model dimensionality (2-D, 3-D, Axisymmetric, etc.)

· Does the model contain rotated nodal coordinate systems?

· Is the model Nonlinear? (see Sample HTML Report)

· Is the model Non-conservative? (see Notes on Unique model features below)

· Actual active DOF for the model

Nonlinear and Load Step Summary

· All sources of nonlinearity are listed

o Large Deformation

o Stress Stiffening

o Plasticity

o Viscoplasticity

o Creep

o Hyperelasticity

o Viscoelasticity

o Nonlinear elasticity

o User material laws

o Cast iron material

o Concrete material

o Gasket material

o Contact (with or without friction)

o Most Nonlinear Control Settings

o Most Load Step Options

o Nonconvergence/termination Settings

o Convergence Criteria

Finite Element Model Diagnostics

§ Element, Type-specific Information

o # of superelements

o # of contact elements (saved as component CAEGCONT, see Appendix A)

o # of pretension elements

o # of p-elements

o # of gasket elements

o # of mesh elements (saved as component CAEGM200, see Appendix A)

o # of surface effect elements (saved as component CAEGSURF, see Appendix A)

o # of shell elements (saved as component CAEGSHEL, see Appendix A)

o # of axisymmetric elements

o # of harmonic elements

o # of composite elements

o # of explicit (LS-DYNA) elements

o # of lumped mass elements

o # of 1-D elements (saved as component CAEG1D, see Appendix A)

Notes on unique model features:

In the MC software, the model is classified as linear or nonlinear on the basis of the following model features/characteristics:

· Large deformation effects are active (see NLGEOM command)

· Stress-stiffening effects are active (see SSTIF command)

· Nonlinear material properties are present (regardless of use)

· Nonlinear element types are defined (regardless of use)

MC also examines the model to report conservative versus non-conservative behavior. This check is done assuming that sources of non-conservative behavior include follower forces in an analysis allowing large deformation, the presence of plasticity, viscoplasticity, viscoelasticity, creep, or the presence of potential frictional contact. Other energy dissipative sources of non-conservative behavior in dynamic problems, such as damping (including discrete damping options for elements LINK11, COMBIN14, COMBIN37 and COMBIN40) are not included in this categorization. In general, non-conservative loadings indicate that the solution is path dependent. In such cases, the model must be subjected to the loads in the sequence they would be applied in actual service.

You can easily move throughout the HTML report using hyperlinks between each report section and the table of contents. Plots that may be included in the HTML report are shown in miniature form or “thumbnails” that are expandable by clicking on the plot.

The HTML report contains separate sections and summary information as follows:

General Information -

Jobname

ANSYS^â Revision Number

ANSYS^â Update Number

Date

Computer System Type

Finite Element Model Units

Title

Number of ANSYS Errors During Checking

Solid Model Entity Summary -

(See Solid Model Checking)

Solid Model Diagnostic Information -

(See Solid Model Checking)

Finite Element Model Information -

Finite Element Model Entity Summary:

	Largest Number	Number Defined	Number Selected
Element Types
Unsupported Element Types
Real Constant Sets
Material Property Sets
Nodes
Elements
Unsupported Elements
Coupling
Constraint Equations

Supported Element Types (by Library name)

Basic Material Properties Used by Selected elements (evaluated at TREF if temperature dependent) and note as to whether nonlinear properties are defined for each used material.

MODE and ISYM values (Fourier components), if Harmonic elements used

Load and Boundary Condition Summary (based on the entire model):

Solid Model Boundary Condition Counts:

Imposed Displacements on keypoints, lines, areas

Forces & Moments on keypoints

Pressure loads on lines, areas

Imposed temperatures on keypoints, elements

Finite Element Model Boundary Condition Counts:

(after transfer of Solid Model boundary conditions)

Imposed Displacements – UX, UY, UZ ROTX, ROTY, ROTZ

Applied Forces – FX, FY, FZ

Applied Moments – MX, MY, MZ

Imposed temperatures on nodes, elements

Applied pressures on elements

Uniform temperature

Reference temperature

Inertia Loads:

	X	Y	Z
Linear Acceleration
Angular Velocity (Global CS)
Angular Acceleration (Global CS)
Reference CS Location
Angular Velocity (Ref. CS)
Angular Acceleration (Ref. CS)

Component Inertia Loads:

	X	Y	Z
Inertia loads on component
Angular Velocity Components
Reference coord system origin
Angular Acceleration Components
Reference coord system origin

Note:

If the same elements exist in more than one component with applied inertia loads then the an error will be reported. Elements that are in multiple components with inertia loading will be stored in component CAEGSHRE

Basic Finite Element Solution Information -

Analysis Type

Equation Solver

ANSYS^â Model Dimensionality

Rotated Nodal Coordinate Systems

Nonlinear Model

Non-conservative Model

Active DOF in Model

Nonlinear and Load Step Summary -

Nonlinear Behavior:

Geometric Effects - Large Deflection, Stress Stiffening

Material Effects - Plasticity, Creep, Viscoplasticity, Cast Iron,

Concrete, Hyperelasticity, Viscoelasticity, Nonlinear Elastic,

Gasket material, User-defined material

Nonlinear Element types

Number of Contact Elements

Materials with MU defined (Coefficient of friction)

Nonlinear Solution Controls:

Newton-Raphson Key (NROPT)

Solution Controls Key (SOLC)

Line Search Key (LNSRCH)

Automatic Time Stepping Key (AUTOTS)

Predictor (PRED) load step & substep flags

Load Step Options:

Step Boundary Conditions (KBC)

Number of Substeps (NSUB), Minimum Substeps, Maximum Substeps

Number of Equilibrium Iterations (NEQIT)

Stiffness Matrix Reuse Key (KUSE)

Convergence Settings:

Non-convergence (NCNV) KSTOP, DLIM, ITLIM, ETLIM, CPLIM

CNVTOL Force Criterion & Norm

CNVTOL Moment criterion & Norm

Finite Element Model Diagnostic Information -

Finite element model diagnostic information is listed for all items checked. The HTML report includes a summary and any warnings or errors for each item in the section titled Finite Element Model Diagnostics (See Sample HTML Report). Next to each warning in the HTML report is a HELP link. If the user clicks on the HELP link, the appropriate section of this users manual will be displayed. Note: this link will not be available if you send this report to someone else that does not have access to the Users Manual installed on your computer system.

Troubleshooting models

MC uses standard and modified versions of ANSYS^â commands to perform the checking and create the HTML report. If such commands generate an ANSYS^â error, MC may, or may not, trap such an error. For instance, if the mesh compatibility test is being done with a model that has very high node and element numbers, ANSYS^â may run out of memory and abort the operation and hence the mesh compatibility section of the HTML report will be incorrect. After the checks have been performed, review the General Model Information section of the HTML report and if the Number of ANSYS Errors During Checking is greater than zero, review the error file (caegrpt.err) and search for the word ERROR to determine the nature of the error(s). If an error occurs during checking, the ‘GLOBAL MODEL INFORMATION’ title of this section of the HTML report will show in the color RED.

There are several areas of checking that can be very compute intensive. These checks may run for a long period of time and may appear to ‘hang’ the software or place it in a suspended state. If MC is being run interactively, message windows appear that indicate what checks are currently being performed. The checks generally fall into two categories, solid model checks and finite element model checks. Let’s address each category for possible long run times.

Solid model checks

The making of solid model parts is usually a very fast and robust operation. Small Entity checks and the Volume/Mass summary computation, however, are much more compute intensive and rely on the ANSYS^â commands ASUM and VSUM to calculate the geometric properties of the selected solid model entities. The ASUM and VSUM computations, in turn, rely on ANSYS^â being able to form a tessellated (faceted) approximation of the geometry. If the user imports complex CAD geometry the tessellation operation may take a long time to complete or could fail. If you are trying to determine whether the MC checking software has a bug in solid model checking, or the corresponding ANSYS^â operation is the culprit, select the same solid model entities and issue the VSUM and ASUM commands in sequence (without using MC). If ANSYS^â reports the volume and area for the selected entities, then MC has a bug. Otherwise, the problem resides in the ANSYS^â software or with the construction of the original solid model. The number of facets used in the tessellated model, in general, determines the speed and accuracy of such calculations. In some instances, a model that cannot be tessellated with coarse faceting will tessellate with a finer setting (see ANSYS^â /FACET command). Some control of this process is available through the use of the user-defined variable, _caegfac. See Appendix B for details. Users have also reported cases where the accuracy of the mass or volume calculation is poor regardless of the facet setting. Again, the use of the ASUM or VSUM command will determine whether MC is reporting an incorrect value or the ANSYS^â program is calculating the value with less accuracy than expected.

Finite element model checks

The compute-intensive calculations associated with the finite element model checks are the Net Load and FEM Mass summaries. Both calculations rely on a modified version of the ANSYS^â inertia relief feature (see the IRLF command) that, in turn, requires partial solutions (using a modified version of the ANSYS^â PSOLVE feature) to be done in the Solution processor. The PSOLVE feature is only available for the products ANSYS^â/Multiphysics, Mechanical and Structural. The Net Load and FEM Mass summary checks are not available for the ANSYS^â/Professional or PrepPost products.

If the model causes a PSOLVE failure, the net load and mass summary computations will also fail. A simple example that could cause failure is a missing real constant or material property set that is needed by the selected elements. While these simple problems are captured by MC and noted in the HTML report, there are more complex situations that are not captured by MC and could result in a PSOLVE failure. However, if the HTML report indicates a PSOLVE failure or if MC hangs during the computation of the net load and mass summary, please review the file ceagrpt.err and search for the word “ERROR”. The ERROR message line(s) are the ANSYS^â solution error messages during the PSOLVE and a quick review of the error messages will usually provide enough information so that an appropriate model correction can be made. We have seen instances (when the error reported during the PSOLVE has to do with some type of record size) where the initial PSOLVE fails and if you simply run MC again, the PSOLVE works and hence the load and mass summary are produced.

Appendix A: Components Created by MC

Components that may be created by the checker:

CAEGCEQN - selected nodes involved in constraint equations, used if the model has DOF mismatch and constraint equations.

CAEGELB - selected elements at start of routine.

CAEGEL - selected, supported elements.

CAEGNODE - selected nodes.

CAEGND - nodes associated with the selected, supported elements.

CAEGUN - unused nodes, i.e., not attached to elements.

CAEGMIS - nodes with DOF mismatch.

CAEGMISN - nodes with DOF mismatch and no constraint equations.

CAEGNCCP - non-coincident nodes in coupled set, tolerance defaults to 1.0E-6. Tolerance can be changed by defining the variable _caegcpt before running MC. See Appendix B.

CAEGNPCP - nodes with nonparallel nodal coordinate systems in coupled set.

CAEGNODT - nodes checked in the temperature check.

CAEGNOMT - if only some of the nodes have temperatures, the temperature check makes this component of nodes without temperatures.

CAEGUDIS - nodes having imposed displacements that have no corresponding DOF (unless supplied by a superelement).

CAEGUFOR - nodes having applied forces/moments that have no corresponding DOF (unless supplied by a superelement).

CAEGUFC - nodes having imposed displacements/applied force/moment conflicts.

CAEGUDF - nodes having displacements/loads that have no corresponding DOF.

CAEGCEN - nodes in constraint equations that produce warnings (from ANSYS routine CECHECK).

CAEGASM - assembly of the original selected entities. Used to return the model to its original state after checking.

CAEGKP - selected keypoints.

CAEGLN - selected lines.

CAEGAR - selected areas.

CAEGVL - selected volumes.

CAEG1D - 1-D elements in the model (including contact elements): Element Types 1,3,4,7,8,10-12,14,16-24,26,27,37-40,44,51,52,54,59-61,180,188,189. Also includes the lumped mass element (MASS21).

CAEG1E - isolated elements (not connected to any other element).

CAEGCONT - contact elements in the model (does not include COMBIN40s): Element Types 12,26,48,49,52,169-174,178

CAEGELET - elements checked in the temperature check, elements types that do not take eleme