FEM: EquationElasticity
|
|
| Menu location |
|---|
| Solve → Equation elasticity |
| Workbenches |
| FEM |
| Default shortcut |
| None |
| Introduced in version |
| - |
| See also |
| FEM tutorial |
Description
De completat
For info about the math of the equation, see the Elmer models manual, section Linear Elasticity.
Usage
- Add an
Elmer solver.
- Select it in the Tree View.
- There are several ways to invoke the command:
- Press the
Elasticity Equation button.
- Select the Solve → Mechanical Equations →
Elasticity Equation option from the menu.
- Press the
- Change the equation's solver settings or the general solver settings if necessary.
Note: For analyses of nonlinear elasticity you must use the Deformation equation (introduced in 0.21). The Elasticity equation is only for linear elasticity.
Note: If you use more than one CPU core for the solver (introduced in 0.21), you cannot use the default solver settings. However, using just one CPU and the default solver settings is in many cases faster than using several CPUs because the elasticity solver is only fast when DateLinear Solver Type is set to Direct (the default, described here). For multi-CPU solving one can only use the DateLinear Direct Method MUMPS. However, MUMPS is not freely available as a direct download.
Solver Settings
For the general solver settings, see the Elmer solver settings.
The elasticity equation provides these special settings:
- DateCalculate Pangle: If the principal angles should be calculated.
- DateCalculate Principal: If all stresses should be calculated.
- DateCalculate Strains: If strains will be calculated. This will also calculate the stresses, even if DateCalculate Principal or DateCalculate Stresses is
false. - DateCalculate Stresses: If stresses should be calculated. Compared to DateCalculate Principal the Tresca yield criterion and the principal stress will not be calculated.
- DateConstant Bulk System: See the Elmer manual for more info.
- DateDisplace Mesh: If mesh can be deformed. This is by default
trueand must be set tofalsefor eigenfrequency analyses. - DateFix Displacement: If displacements or forces are set. thereby DateModel Lumping is automatically used.
- DateGeometric Stiffness: Considers the geometric stiffness of the body.
- DateIncompressible: Computation of incompressible material in connection with viscoelastic Maxwell material and a custom DateVariable.
- DateMaxwell Material: Compute the viscoelastic material model.
- DateModel Lumping: Uses model lumping.
- DateModel Lumping Filename: File to save the results from the model lumping.
- DateStability Analysis: If
trueDateEigen Analysis becomes a stability analysis (buckling analysis). Otherwise a modal analysis is performed. - DateUpdate Transient System: See the Elmer manual for more info.
- DateVariable: The variable for the elasticity equation. Only change this if DateIncompressible is set to
truein accordance to the Elmer manual.
Eigenvalues:
- DateEigen Analysis: If an eigen analysis should be performed (calculation of eigenmodes and eigenfrequencies).
- DateEigen System Complex: Should be
trueif the eigen system is complex. it must befalsefor a damped eigen value analyses. - DateEigen System Compute Residuals: Computes residuals of the eigen value system.
- DateEigen System Damped: Set a damped eigen analysis. Can only be used if DateLinear Solver Type is Iterative.
- DateEigen System Select: Selection of which eigenvalues are computed. Note that the selection of Largest* cause an infinite run for recent Elmer solver (as of August 2022).
- DateEigen System Tolerance: Convergence tolerance for iterative eigensystem solve. The default is 100 times the DateLinear Tolerance.
- DateEigen System Values: The number of the highest eigenmode that should be calculated.
Equation:
- DatePlane Stress: Computes solution according to the plane stress situation. Applies only for 2D geometry.
Analysis Feature Information
The elasticity equation takes the following analysis features into account if they are set:
Fixed boundary condition
Displacement boundary condition
Force load
Initial temperature condition
Pressure load
Gravity load
Spring
Note
- Except for calculations in 2D, for all the above analysis features it is important that they act on a face. Features in 3D set to lines or vertices are not recognized by the Elmer solver.
Eigenmode Analysis
To perform an eigenmode analysis (calculation if the eigenmodes and eigenfrequencies), you need to
- Set DateEigen Analysis to
true - Set DateDisplace Mesh to
false - Set DateEigen System Values to the highest number of eigenmodes you are interested in. The smaller this number the shorter the solver runtime since higher modes can be omitted from computation.
- Add a fixed boundary condition and set at least one face of the body as fixed.
- Run the solver.
It is highly recommended to use DateLinear Solver Type set to Direct (the default) because this is much faster and the results are more accurate.
Buckling Analysis
To perform a buckling analysis, you need to do the same as for an Eigenmode Analysis, and additionally:
- Set DateStability Analysis to
true
Results
The available results depend on the solver settings. If none of the DateCalculate * settings was set to true, only the displacement is calculated. Otherwise also the corresponding results will be available. If DateEigen Analysis was set to true all results will be available for every calculated eigenmode.
If DateEigen Analysis was set to true, the eigenfrequencies are output at the end of the solver log in the solver dialog and also in the document SolverElmerOutput that will be created in the Tree View after the solver has finished.
Note: The eigenmode displacement vector has an arbitrary value since the result is
whereas is the eigenvector and is a complex number.
- Materials: Solid Material, Fluid Material, Non-Linear Mechanical Material, Reinforced Material (Concrete); Material Editor
- Element Geometry: Beam Cross Section, Beam Rotation, Shell Plate Thickness, Fluid Section for 1D Flow
- Electromagnetic Boundary Conditions: Electrostatic Potential Boundary Condition, Current Density Boundary Condition, Magnetization Boundary Condition, Electric Charge Density
- Fluid Boundary Conditions: Initial Flow Velocity Condition, Initial Pressure Condition, Flow Velocity Boundary Condition
- Geometrical Analysis Features: Plane Multi-Point Constraint, Section Print Feature, Local Coordinate System
- Mechanical Boundary Conditions and Loads: Fixed Boundary Condition, Rigid Body Constraint, Displacement Boundary Condition, Contact Constraint, Tie Constraint, Spring Boundary Condition, Force Load, Pressure Load, Centrifugal Load, Gravity Load
- Thermal Boundary Conditions and Loads: Initial Temperature, Heat Flux Load, Temperature Boundary Condition, Body Heat Source
- Overwrite Constants: Constant Vacuum Permittivity
- Mesh: Mesh From Shape by Netgen, Mesh From Shape by Gmsh, Mesh Boundary Layer, Mesh Refinement, Mesh Group, Erase Elements, FEM Mesh to Mesh
- Solve: Solver CalculiX, Solver Elmer, Solver Mystran, Solver Z88; Mechanical Equations: Elasticity Equation, Deformation Equation; Electromagnetic Equations: Electrostatic Equation, Electricforce Equation, Magnetodynamic Equation, Magnetodynamic 2D Equation, Static Current Equation; Flow Equation, Flux Equation, Heat Equation, Solver Job Control, Run Solver
- Results: Purge Results, Show Result, Apply Changes to Pipeline, Post Pipeline From Result, Pipeline Branch, Warp Filter, Scalar Clip Filter, Function Cut Filter, Region Clip Filter, Contours Filter, Glyph Filter, Line Clip Filter, Stress Linearization Plot, Data at Point Clip Filter, Calculator Filter; Filter Functions: Plane, Sphere, Cylinder, Box; Data Visualizations: Create Lineplot, Create Histogram, Create Table
- Utilities: Clipping Plane on Face, Remove All Clipping Planes, FEM Examples; Clear FEM Mesh, Display Mesh Info
- Additional: Preferences; FEM Install, FEM Mesh, FEM Solver, FEM CalculiX, FEM Concrete; FEM Element Types
- Getting started
- Installation: Download, Windows, Linux, Mac, Additional components, Docker, AppImage, Ubuntu Snap
- Basics: About FreeCAD, Interface, Mouse navigation, Selection methods, Object name, Preferences, Workbenches, Document structure, Properties, Help FreeCAD, Donate
- Help: Tutorials, Video tutorials
- Workbenches: Std Base, Assembly, BIM, CAM, Draft, FEM, Inspection, Material, Mesh, OpenSCAD, Part, PartDesign, Points, Reverse Engineering, Robot, Sketcher, Spreadsheet, Surface, TechDraw, Test Framework
- Hubs: User hub, Power users hub, Developer hub