Finite Element Analysis

1. Finite Element Analysis Introduction using MSC.Patran and MSC.Nastran

2. Overview • Patran basics • Model building process • Submitting the analysis • Results basics • Example problems

3. Patran basics • Patran is a general-purpose Pre- and Post processor. It can create models for a large number of analysis codes • Pre-processing is the process of building a mesh, applying material properties, loads and boundary conditions and writing it out in the format that the finite element solver needs it. • Post-processing is simply looking at the results of an analysis (Deformation plots, contour plots, graphs etc)

4. Patran basics Menu bar Quick-icons Form area Main workflow icons Model window Command line History window

5. Patran basics • After opening patran, create or open a DB file. This is the main Patran model file and is a kind of database file. • When a new model is created, a form is shown where the solver / analysis type is selected and a model sizing parameter is chosen. The default of 10 is OK for typical models built in mm. Use 0.01 for the same model in SI

6. Patran basics The basic workflow in Patran is: • Create / Import geometry • Mesh the geometry • Apply loads / Boundary conditions • Create material properties and apply to the elements • Submit the analysis • Import the results and post-process The main workflow icons are used to perform these steps.

7. Patran basics • Forms follows the same basic layout for all forms. For forms that need to perform different tasks, a series of drop-down lists at the top is used to change into the mode required. • The actions for these drop-down lists are Action/Object/Method or Action/Object/Type • Action: What do you want to do (Create / delete / transform / modify / renumber etc) • Object: On what do you want to perform this action (Curve / Surface / Solid / Element / Node etc) • Method: What method do you want to use to perform this action (Extrude / revolve etc.) • Type: More details on the Object to be operated on (Element uniform / Element variable etc) • This makes it easy to find a specific feature in Patran

8. Patran basics

9. Patran basics Some comments about the interface: • No action is taken until the “Apply” button is selected • An “Auto execute” tick-box means that Patran automatically presses the “Apply” button for you if you select something with the mouse • “Cancel” is usually used to close a form • When a new command is given to Patran, the model is first saved and the command then executed. This means that you never lose more than one step even with a power-failure. The downside is that only the last command can be undone (because it is not yet saved)

10. Model building process • The first part in building a model is to get geometry available so that a mesh can be generated. Most commonly the model comes from a CAD package. The following types of CAD files are supported: • ACIS (Used by Autocad) • Parasolid (Used by Unigraphics, Solid Edge, Solid Words and a couple of others) • Catia • Pro Engineer • Unigraphics • IGES • STEP • Patran has it’s own geometry engine as well as the Parasolid geometry engine built in. Therefore, the geometry that gives the least amount of problems is Parasolid, although ACIS, CATIA and Pro Engineer import interfaces also works very well. • It is possible to completely build a model in Patran without the use of a CAD package. However, Patran was never intended as a CAD tool. Creating geometry in Patran invariably takes longer than in most CAD packages. Also remember that Patran until recently was not parametric at all, and is only slowly getting parametric geometry now.

11. Model building process • After geometry exists, the Finite Element model creation process can start. The workflow mentioned earlier is not a fixed method of working: As long as geometry exist the sequence can be changed at will • Patran can apply loads, boundary conditions and properties to either Geometry or to FE entities (nodes / elements). Applying it to the geometry means that Patran will map it to the elements at the time of submitting the analysis • This means that you can re-mesh the model without having to update every load, BC and material property.

12. Model building process • Creating a mesh depends on the class of element to be used and the level of control over the mesh required. On the Elements menu, set it to Create / Mesh / [Entity type] where [Entity type] can be Curve, Surface or Solid.

13. Model building process • Create / Mesh / Surface gives two options for the meshing Algorithm: Isomesh and Paver. • IsoMesh is only allowed on 3- or 4-sided surfaces (Green surfaces). It transforms this surface onto a square or triangular surface, “subdivide” this mesh to get elements and transforms back to the original surface. • Paver is valid for all types of surfaces (Green and Magenta). It starts “Paving” at the edges and then continues “paving” towards the inside until the area is filled. • Both meshing methods can create Tri- or Quad elements. • To control a surface mesh, it is possible to create a “Mesh-seed” (Create/Mesh-seed). This is a “constraint” on the meshing algorithm that forces it to place a certain number of nodes along a certain edge with a certain spacing. • Uniform seeding is the most commonly used because it makes meshing non-congruent surfaces easier. • A “One way bias” seed goes from coarse to fine or fine to coarse. It is useful to force smaller elements at a stress-concentration.

14. Model building process • Create / Mesh / Solid also has two meshing options: • IsoMesh is similar to the one for surfaces. It can generate Tet, Penta or Hex elements, but ONLY on blue solids (Solids that have 6 4-sided faces) • “Tetmesh” as the name indicates is for creating Tet elements. It can mesh any kind of solid geometry (Blue or white solids) • Controlling the mesh for a solid model is more complex. Mesh seeds can still be used on edges, but that does not mean that the face between the edges will get the same element length. To force a certain mesh-size on a face, two methods exist: • a “Mesh control” can be applied to force a local mesh size. I don’t recommend it because it is easy to forget about them and have difficulty trying to mesh the solid with different parameters. • Create a Tri-mesh of the same order as the Tet-mesh that you plan to apply. When you then mesh with Tet-elements, elements will be created with faces that match the surface elements. Then delete the Tri-mesh.

15. Model building process • If two separate pieces of geometry next to each other is meshed, they may have nodes at the same location in space but they are NOT connected by default. To connect them, use the “Equivalence” option. It forces the elements to share the boundary nodes instead of having duplicate nodes. Remember, if they don’t share nodes, the elements are not connected! • To check that the mesh is connected, use the “Verify / Element / Boundaries” option. It will show where there are element edges that is not shared. In other words it tells you where there are elements that are not connected to others. If the model is correct, there should only be lines at the boundary of the model. Correct wrong

16. Model building process • Applying loads and boundary conditions is relatively straightforward: • Choose the load-type • Give the load a unique name (without spaces) • Choose to what elements (1D / 2D / 3D) the load is applied to if applicable • Go to “Input data” to fill in the load value. The value may be a scalar or a vector (more on vectors later). Select “OK” • Go to “Select application region”. Select whether you want to apply the load to FEM or Geometry. Select the entities to apply the load to and press the “Add” button. Repeat this selection and “Add” until all the entities are in the “Application region”. Press “OK” • Press “Apply” • Check that the Load / BC has been added to the “Existing sets”. If not, either there was an error (an error window would appear with some kind of message), or you did not press apply. • To check what the properties was of a specific load / BC, select it in the “Existing sets” (Typing it’s name is NOT good enough). It will then fill in it’s data in the name, “Input data” area and “application region.

17. Model building process • Applying materials to a mesh is a two-step process: • First, create a material. Note that the materials do not have an option to link them to any elements: They are simply made available to be used on the properties menu. • To create a Material:On the materials menu, select Create / [Property type] / Manual input. [Property type] is: • Isotropic for materials that do not exhibit varying properties in different directions. Typically used for metals. Required properties is two of Modulus of elasticity (E), Shear modulus (G), or Poisson (ν). Density is needed if either inertial loading (gravity / rotational velocity) is applied, or if a type of dynamic analysis is to be performed • Orthotropic for materials that has properties that can be defined be specifying a different stiffness in 3 orthogonal directions. A layer of composites is typical of this. • Anisotropic has more terms for the material stiffness than even Orthotropic and can have for example coupling between membrane stress and bending. A complex composite lay-up has this kind of behavior, although it will more commonly be set up using the following option • Composite is used to define material properties for a material that is built up in layers of materials that has already defined • Fluid is used to specify material properties for acoustic analysis • Select “Input material properties” and fill in the required data. Press OK and Apply

18. Model building process • To apply the material properties to a mesh, go to the properties menu: • Create / [Dimensionality] / [Type of element] • [Dimensionality] can be from 0D to 3D. • [Type of element] vary for each dimensionality. Most commonly used is: • 0D: • Mass element • Grounded spring - Has a stiffness in a specific direction that is between one node and ground. Used to model foundations that are not perfectly stiff • 1D: • Beam • Rod – Truss element • Bush – spring element that can define different stiffness for each DOF as well as Damping between two nodes. • 2D: • Shell – An element that acts in 3D space but which is modeled without nodes in the thickness direction. Have membrane, shear and bending stiffness by default • 2D solid: Options are “Plane Strain” or axi-symmetric. They are defined in 2D but define a thick component. • 3D: Only option is “Solid”.

19. Model building process • Select the type of property to apply and go to “input properties”, fill in the properties and press “OK”. The smaller the dimensionality of the element is, the more properties is needed: • 3D: Only a material is needed • 2D: A material and a thickness • 1D: A material, Cross-sectional area, Inertia values, direction to determine in which direction the normal direction for the element is (i.e. what is the orientation of the beam) • 0D: Mass properties (Mass and Inertia) or Stiffness for each direction • Select the geometry or elements to which to apply and press “Add” to fill in the “Application region”. Select “Apply” to generate the properties • .

20. Model building process • Going to the “Load Cases” menu is only needed if you plan to run multiple load-cases. • A Load Case is a collection of loads / BCs that is to be applied to the model. In other words it is a loading condition you want to analyze. By default, a load case called “default” is created when you create a new Patran DB, and all loads / BCs are added to it when you create them. • Creating a load case is simple: • Give it a name • On “Input data”, select the loads and BCs that should be used and “OK” then press “Apply” • Check that the load case name is displayed in the “Existing Load Cases” data box.

21. Submitting the analysis • You are now ready to start the analysis. On the analysis menu, select Analyze / Entire model / Full run. The “Job name” is what the Nastran model will be called (it defaults to the Patran model file-name) as well as what the results-file is called. • On translation parameters: • Switch off “Print”. The “print” file is the .F06 file, and having “print” on will write all results to this text file as well as to the normal results file. This will then be a HUGE file and make it difficult to scan it for errors. More on the F06 later. • Choose either XDB or OP2 for output. • XDB is a database format file that is not imported into Patran: When results are created, it accesses this file. • OP2 is imported into Patran, so the file can be deleted after importing results. The Patran DB can become very large if multiple load cases are read in in this fashion. • The rest of the settings are OK, so select “OK” • Use “Solution type” if you don’t plan to run a linear static analysis

22. Submitting the analysis • Make a “Direct text input” in the Bulk data section: “Param, PRGPST, NO” to not print the grid-point singularity table to the F06 file, and select “OK”. This will reduce the size of the F06 significantly.

23. Submitting the analysis • Go to “Sub cases” to change settings for any load case to be run. This is needed to change the results requested (default is stress, reaction force and displacement). For non-linear analyses, load increment info is set here. For Transient analysis types, time steps or number of modes are set here. [A sub case is a load case with extra info about settings for the load case] • Select the sub cases to be run on the “Sub case select” menu, OK and Apply to submit the analysis. • If all goes according to plan, a Command window will open that shows that Nastran is running. This window will stay open for at least a couple of seconds (up to several hours depending on the model size). When the analysis has completed, check the F06 file for errors. Search for “FATAL” in this file. If it’s there, the results file will contain NO RESULTS! • To Access the results: • On the Analysis menu, select “Access results” / [“Attach XDB” or “Read OP2”] / “Result entities”. Select the results file and press “Apply”. The results should now be available on the “Results” menu.

24. Results basics The most common result plots used are: • Displacement - showing deformed shape) • Fringe - showing contours • Quick Plot - combines the a Fringe and Displacement plot. It has less options than Fringe / Displacement plots, so is used to generate the first impressions of the results Other result types available are: • Marker – Used mostly to generate vectors • Cursor – Used to show a value at a specific node location • Contour – Create contour lines • Graph – Create a graph of Result vs. Location or time • Animation – Seldom used: Can animate from Fringe / Displacement / Quick plot • Report – Used to write results to a file • Results – Create a new result that is either a scaled version of another, or a summation of a series of load cases (valid only for linear analyses) • Freebody – Generates free-body diagrams. Must request extra results information during the analysis to be able to perform this step.