The following describes the intended work flow and some general tips for going through the steps to run a simulation using BasicFEA.
BasicFEA will read the unit system of most geometry files on import and set the working units appropriately. If you get the message shown below it means that BasicFEA was not able to determine the unit system from the geometry file. The default units in the BasicFEA environment are set to mm tonne K N MPa so any new material, load or mesh size are all defined in those units. It is important to match the geometry to the BasicFEA environment before continuing.
A good first step when starting an analysis is to measure the model. This will give you a feel for the size and is a good check to make sure the units make sense. Click the icon on the toolbar to enter into dimension mode. While in this mode you can simply view the global X,Y,Z bounding box or select your own points to measure.
BasicFEA will read the units from most imported geometry, but if unable to determine the units, or if they are in a set of unsupported units, the Scale model only option in the BasicFEA browser allows you to easily convert only the geometry from units -> units. Right-click anywhere inside the BasicFEA browser and click the Scale model only option.
Switching units in BasicFEA will update the entire model, so use the Scale model only option to match your model to the working units listed at the top of the browser. Separate scale factors can also be applied to the geometry only in order to get a matching set of units between geometry and the rest of the BasicFEA environment.
Analyzing parts made of sheet metal can sometimes be challenging due to the nature of the thin, solid geometry. The solution for these types of parts is to find the “midsurface” of the 3D geometry and operate on that with 2D shell elements that carry the representative thickness. Depending on the type of geometry you are importing, BasicFEA has the following options for Solid to Shell midsurfacing:
3D Solid CAD
2D Surface CAD
Solid parts in the BasicFEA browser are represented by the icon and have their material displayed as a child. Shell parts are represented by the icon and have the material child along with a thickness editor that changes the thickness for the entire part.
Meshing is something that is done behind the scenes with BasicFEA. Mesh size and type are automatically generated on import and the elements are added right before the analysis is submitted.
If you want to change the mesh settings, that ability is offered on the global scale and for each individual part.
None of the setup for BasicFEA is dependent on a mesh. HyperMesh offers a great deal of meshing options and techniques. At anytime a model generated in BasicFEA can be brought back into HyperMesh and meshed separately by clicking the icon. Moving from BasicFEA to the HyperMesh client ensures that you have a running model to start with before continuing with advanced pre-processing.
BasicFEA supports two types of contact: tied and sliding. To create a contact choose New Tied Contact or New Sliding Contact from the Contacts right-click context menu. The contact definition will be automatically created, leaving you to choose the main and secondary parts. Choose from the list of parts or pick on the screen.
At any time, tied contact can be switched to sliding contact, and vice versa. You can input friction values for sliding contacts. Tied contacts do not have friction.
Auto-contact is a simple way to define contact throughout your model. Selecting Auto-contact from the Contacts folder will search through each part in your model and define a tied contact on parts within an automatic volume based tolerance. It is recommended to review each contact before submitting an analysis. After running an auto-contact, the newly created tied contact pairs can be changed, deleted or switched to sliding to perform a non-linear sliding contact analysis.
BasicFEA supports the following loadstep types:
The Linear Static loadstep type in BasicFEA allows you to load your model in the linear space using constraints and distributed loads applied to geometry.
Frequency ranges and the number of desired roots are all controlled within the details of each Normal Modes loadstep. Without a constraint defined in the loadstep a free-free boundary condition is assumed, and by default the first six modes found will be the rigid body modes.
Small deformation theory is used in the solution of nonlinear problems, similar to the way it is used with linear static analysis. Small deformation theory means that strains should be within linear elasticity range, and rotations within small rotation range. This also means that there is no update of gap/contact element locations or orientation due to the deformations. They remain the same throughout the nonlinear computations.
Large deformation theory is used in nonlinear problems by enabling the large displacement option (LGDISP) which allows for non-linear load-response relationships and structural large displacements. Strains can go beyond the linear elastic range and into the plastic region given a valid material definition and rotations can be larger within the range.
Continual subcase allows you to select a previous nonlinear subcase to continue the solution from one subcase to another.
The same loading is available for a Non-Linear Quasi-Static loadstep that is available for linear statics. Before running the analysis make sure to choose which contact definitions are sliding and which are tied. While running a Non-Linear Quasi-Static loadstep containing sliding contacts a search is conducted for open and closed contact based on the loading conditions. Tied contacts simply tie two parts together. If a sliding contact is defined for a linear type loadstep, it will act as a tied contact.
BasicFEA allows for the selection of both linear static and non-linear quasi-static subcases. Additionally, you can select up to 10 total subcases for cycling between. There is also the ability to specify time history data through direct input or import. Additional options are available within the BasicFEA browser, although not every solver option is covered. For full control of the fatigue loadstep, switch to the OptiStruct user profile, and consult the OptiStruct User Guide for more information.
A Common Loads folder is available in the BasicFEA browser by default. Loads in this folder will be applied to all loadsteps.
Post-processing in BasicFEA is limited to what exists in HyperMesh post. Producing simple stress and displacement contour and vector plots is available in the Contour and Vector Plot panels. For simple animations and deformed shapes, the Deformed panel allows you some flexibility.
If the post-processing is not sufficient in BasicFEA, clicking the icon takes you to the HyperView client, which may be more appropriate for advanced post-processing and report generation.