Donate

FEM Mesh to Mesh

Solver Elmer

FEM

Description

Enables usage of the CalculiX solver. It may be used for:

1. Setting analysis parameters
2. Selecting working directory
3. Running the CalculiX solver

introduced in 1.1: If the Result object CalculiX FEM preference is enabled, a refactored CalculiX solver object is added to the Analysis container by this command. It has a redesigned task panel (works like task panels of the meshers - press Apply to run the analysis), doesn't generate the CCX_Results objects (only the results pipeline is generated) and supports electrostatic analyses.

Usage

1. A SolverCcxTools solver object is created automatically with the creation of an Analysis container if CalculiX is selected as the default solver in the General FEM preferences.
   To create it manually, do one of the following:
   • Press the Solver CalculiX button.
   • Select Solve → Solver CalculiX from the menu.
   • Press the shortcut keys:
     • 1.0 and below: S X
     • 1.1 and above: S C
2. Optionally change the properties of the SolverCcxTools solver object in the Property View.
3. Double click the SolverCcxTools solver object.
4. Select the Analysis type.
5. Click the Write .inp file button.
6. Click the Run CalculiX button.

Options

Click the Edit .inp file button to display and edit the CalculiX input file manually before running the analysis. In that case it can be useful to set the ÚdajeSplit Input Writer property to true.

Properties

This section has been updated for version 1.2.

Default values can be set in the menu Edit → Preferences → FEM → CalculiX

• ÚdajeAnalysis Type:
  • static - static stress analysis
  • frequency - modal (natural frequency) analysis
  • thermomech - thermo-mechanical analysis
  • check - no calculation, performs input deck checks
  • buckling - linear buckling analysis introduced in 0.20
  • electromagnetic - electromagnetic analysis (available only for the refactored CalculiX solver object) introduced in 1.1

• ÚdajeAutomatic Incrementation:
  • true - incrementation control will be automatic
  • false - automatic incrementation control will be switched off by the DIRECT parameter

• ÚdajeBeam Reduced Integration - introduced in 1.0:
  • true - uses beam elements with reduced integration (B31R or B32R), required when pipe beam section is used, can also make it possible to obtain accurate results with plasticity
  • false - uses regular (fully-integrated) beam elements

• ÚdajeBuckling Accuracy - introduced in 1.1: defines the accuracy of buckling eigenvalue evaluation. In most cases it can be left with the default value (0.01) but sometimes it might be necessary to lower it (e.g. to 0.0001) to capture the first eigenvalue.

• ÚdajeDisplace Mesh - introduced in 1.2: displays true scale deformation of the mesh in the results pipeline without the need for the Warp filter (available only for the refactored CalculiX solver object)

• ÚdajeEigenmode High Limit: Eigenvalues above this limit will not be calculated; Note: if eigenvalues of the model are above the high limit, CalculiX will finish without output

• ÚdajeEigenmode Low Limit: Eigenvalues below this limit will not be calculated

• ÚdajeEigenmodes Count: number of lowest eigenmodes to be calculated

• ÚdajeElectromagnetic Mode - introduced in 1.0: type of the electromagnetic analysis, available only with the refactored CalculiX solver object
  • electrostatic - electrostatic analysis

• ÚdajeExclude Bending Stiffness - introduced in 1.1:
  • true - shell elements are replaced with membrane elements and beam elements are replaced with truss elements
  • false - shell and beam elements are used

• ÚdajeGeometric Nonlinearity:
  • linear - linear analysis will be performed if the model does not contain nonlinear material
  • nonlinear - nonlinear analysis will be performed

• ÚdajeIncrements Maximum: maximum number of increments after which the job will be stopped.

• ÚdajeIterations Control parameter Cutb: defines the second line of CalculiX' advanced iteration parameters. Used if ÚdajeIterations Control Parameter Time Use is set to true.

• ÚdajeIterations Control Parameter Iter: defines the first line of CalculiX' advanced iteration parameters. Used if ÚdajeIterations Control Parameter Time Use is set to true.

• ÚdajeIterations Control Parameter Time Use
  • true - activates ÚdajeIterations Control parameter Cutb and ÚdajeIterations Control Parameter Iter
  • false

• ÚdajeMaterial Nonlinearity:
  • linear - only linear material properties will be included in the analysis
  • nonlinear - nonlinear material properties will be used from Nonlinear mechanical material object

• ÚdajeMatrix Solver Type: type of the solver to solve equation system inside finite element analysis. It may significantly affect calculation speed and memory demands. Suitability depends on your finite element model and available hardware
  • default - automatically selects matrix solver depending on the available solvers (typically it is Spooles)
  • introduced in 1.0: pastix - one of the fastest solvers (along with Pardiso), available (and default) in official builds since ccx 2.18, may still cause occasional issues
  • introduced in 1.0: pardiso - one of the fastest solvers (along with PaStiX) but not open-source, requires a different build of CalculiX (ccx_dynamic) and additional libraries not provided with FreeCAD, more reliable than PaStiX
  • spooles - direct solver with the support of multiple CPUs. The number of CPUs needs to be set in the preferences at Solver defaults → Number of CPU's to use.
  • iterativescaling - iterative solver with the lowest memory demands, suitable if the model contains mostly 3D elements
  • iterativecholesky - iterative solver with preconditioning with and with low memory demands, suitable if the model contains mostly 3D elements

• ÚdajeModel Space - introduced in 1.0: switches between 3D and 2D analyses, the latter require surface geometry on the XY-plane (on the right of the Y-axis in the axisymmetric case) with thickness definition (value ignored in the axisymmetric case) and proper boundary conditions (displacement boundary condition with degrees of freedom X and Y has to be used instead of fixed boundary condition) and in-plane loads applied to edges. CalculiX's 2D elements can be used not only for mechanical but also thermal, coupled and electromagnetic analyses.
  • 3D - three-dimensional solid/shell/beam elements are used
  • plane stress - plane stress 2D solid elements are used
  • plane strain - plane strain 2D solid elements are used
  • axisymmetric - axisymmetric 2D solid elements are used

• ÚdajeOutput 3d: note that CalculiX internally expands 1D and 2D elements into 3D elements to accomplish finite element analysis
  • true - resulting mesh will contain 1D and 2D elements expanded to 3D elements
  • false - results of 1D and 2D elements will be averaged to the nodes of the original 1D or 2D mesh (i.e. a purely bent beam will show 0 nodal stresses due to averaging)

• ÚdajeOutput Frequency - introduced in 1.0: defines the frequency of results writing in increments (the default setting of 1 means that the results are written every increment, setting 2 would save the results every 2 increments and so on), particularly useful for nonlinear and transient simulations, helps reduce the clutter in the tree since currently a pair of results objects (CCX_Results and Pipeline_CCX_Results) is created for each results frame

• ÚdajePastix Mixed Precision:
  • false - mixed precision is not used by the PaStiX solver
  • true - mixed precision is used by the PaStiX solver, may cause issues with results in some cases

• ÚdajeSplit Input Writer:
  • false - write whole input into one *.inp file to be used by CalculiX solver
  • true - split solver inputs into more *.inp files, that can clarify manual editing

• ÚdajeThermo Mech Steady State:
  • true - steady state thermo-mechanical analysis
  • false - transient thermo-mechanical analysis

• ÚdajeThermo Mech Type - introduced in 1.0:
  • coupled - coupled thermo-mechanical analysis
  • uncoupled - uncoupled thermo-mechanical analysis
  • pure heat transfer - purely thermal analysis (*HEAT TRANSFER)

• ÚdajeTime Initial Increment: suggested initial time increment for the analysis step, can be modified by the solver unless Automatic Incrementation is disabled and thus direct incrementation is used (then this is the increment size CalculiX will have to use)

• ÚdajeTime Maximum Increment - introduced in 1.0: maximum time increment size for the analysis step, not used if Automatic Incrementation is disabled and thus direct incrementation is used

• ÚdajeTime Minimum Increment - introduced in 1.0: minimum time increment for the analysis step, not used if Automatic Incrementation is disabled and thus direct incrementation is used

• ÚdajeTime Period: time period of the analysis step

• ÚdajeWorking Dir: path to the working directory which will be used for CalculiX analysis files.

Limitations

When running a CalculiX, you might end up with error 4294977295. This means you don't have enough RAM space. You have then 2 options:

1. reduce the number of mesh nodes, preferably by omitting geometry that is not absolutely necessary for your analysis
2. buy more RAM for your PC

Notes

Original CalculiX documentation can be found at http://dhondt.de/ in the "ccx" paragraph.

Scripting

FEM Mesh to Mesh

Solver Elmer

FEM