Ever get thrown an old NASTRAN model or been asked to convert your model into ABAQUS? Did you spend hours scouring the internet for a free translator? Did you know that ANSYS software came with a translator for FLUENT, CFX, ABAQUS, NASTRAN , STL files and a host of other formats? Well it does and it comes free with most products. It is one of the least known jewels in the ANSYS product family.
FE Modeler is a module developed to handle some of the mesh based capabilities found in Mechanical APDL that don’t really fit into the paradigm of what is now called ANSYS Mechanical. Over the years it has grown to be a very useful tool for translating models, reviewing meshes, morphing meshes, and even converting meshes into geometry that can be re-meshed. In this article we will talk about the translators and quality tools and will address the morphing and geometry-from-mesh tools once R13 comes out in November.
The first thing to know is how to get to this useful tool. On the workbench page, it is in Toolbox under Component Systems with the name Finite Element Modeler. Figure 1 shows where it is located.
Figure 1: Location of FE Modeler Tool
There are a couple of ways to use the tool. The first is to drag it onto a mesh that already exists in your project. This is the best way to proceed if you meshed with Workbench meshing or a system that uses Workbench Meshing (Mechanical, FLUENT, CFX, etc…). You can also connect it to the Setup block on an ANSYS Mechanical system. You can of course connect to an FE Modeler system by right clicking on a mesh and choosing “Transfer Too New… -> Finite Element Modeler” Figure 2 shows some examples of what it looks like once you have connected.
Figure 2: Connecting to a Workbench Mesh or Model
If you are not starting with a Workbench related mesh or model, you can still use the tool. This is the most common method for reading in NASTRAN or ABAQUS meshes. Simply drag and drop the Finite Element Modeler System to a blank spot on the Project Schematic. Once there you can specify your input file in one of two ways: double-click on the Model (brute force, take charge, throw caution to the wind approach) or right click on the Model and choose “Add Input Mesh” (take your time, make sure it is right, no risks approach). And yes, it says “Add” because you can specify multiple meshes, an added bonus. Figure 3 shows an example of what this will look like.
Figure 3: Stand Alone FE Modeler Systems
When you are in the browser dialog you can see the various formats that are supported (Figure 4). These are also summarized in Table 1:
Figure 4: Input Options
Table 1: Supported Input File Summary
|ABAQUS (*.inp)||MAPDL (*.cdb)|
|CFX (*.def, *.res)||NASTRAN (*.bdf, *.dat, *.nas)|
|ANSYS WB Meshes (*.cmdb, *.meshdat)||Mechanical (*.dsdb, *.mechdat)|
|Fluent (*.msh,*.cas)||STL (*.stl)|
|ICEM CFD (*.uns)|
Now you have a mesh defined. The next step is to read it in to FE Modeler. You can do this by double clicking on the model or RMB->Edit. The program will now read in your file, and display a nice animated spinning gear to keep you occupied. The numbers in feedback in the Import Summary (the default view) also update as the file is read.Once in FE Modeler you will see a pretty standard layout for a Workbench application. The tree on the left, Details view on the lower left, and a graphics window. To start with Import Summary will be selected in the tree and a description of what was read in is shown. There is a lot of useful information in this view. Take some time to look at each table and see if it makes sense. Probably the most important table is Table 4. It shows feedback from the import. If the reader ran into any entities it didn’t recognize or any lines it could not read, you will see feedback here. This is important because there often are not one-to-one mappings between programs so some entities will not read in. You will be able to see those in this table. Figure 5 shows the output from reading in a basic test model from a NASTRAN file.
Figure 5: Typical Feedback from Input
Now, if you want to see your model, you can click on other branches in the tree. The Element Types allows you to view by element topology and Bodies will show the contents of a given file. You can also interrogate the mesh, selecting nodes, external faces, or elements and viewing their position. Take a look at the icon bar, it is pretty standard for Workbench and everything is self explanatory. You can see mesh metrics by choosing Insert from the menu and then picking Mesh Metrics. Once it is in the tree, click on it and change the options in the details view. Figure 6 shows the test model and some quality metrics.
Figure 6: Mesh Metrics
The last step is the best part, writing out in the new format that you want. Find the “Target System” drop down at the top of the icon bar, and choose from Mechanical APDL, ABAQUS, NASTRAN, and STL. Then select “Generate Data” in the model tree and the program will create an output file in the format you want. This can take a while for a large model.
Figure 7: ABAQUS Output
If you are an expert in the program you are writing to, you can check this file out and see what is in there. If you like what you see, or don’t care and just want your output file, click on the “Write Solver File” button on the top icon bar. Specify a file name, and you are done.
There is one last important thing to mention. If you want to control your import a little, go back to the project page and click on the model. RMB and choose “Manage Input Meshes”. This will then bring up the outline for the schematic and you will be able to set options for each file you specified for input. (Figure 8) For most files the only things you can change are units, how to group bodies and how to number things.
Figure 8: Options for Inputting of Files
Nothing too complicated, it does what it does and it does it fast. To learn more play with it and read the help. We hope you find this hidden tool as useful as we have in the past.