FEM SolverCalculixCcxtools/ru

Описание

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.

Применение

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 Standard button.
   • Select Solve → Solver CalculiX Standard 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 editor.
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.

Опции

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 ДанныеSplit Input Writer property to true.

Свойства

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

• ДанныеAnalysis 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

• ДанныеBeam 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

• ДанныеBeam Shell Result Output 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)

• ДанныеBuckling 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.

• ДанныеEigenmode 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

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

• ДанныеEigenmodes Count: number of lowest eigenmodes to be calculated

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

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

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

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

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

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

• ДанныеIterations User Defined Incrementations:
  • true - automatic incrementation control will be switched off by the DIRECT parameter
  • false - incrementation control will be automatic

• ДанныеIterations User Defined Time Step Length:
  • true - activates ДанныеTime End and ДанныеTime Initial Step parameters
  • false

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

• ДанныеMatrix 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

• ДанныеModel 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

• ДанныеOutput 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

• ДанныеSplit 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

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

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

• ДанныеTime End: time period of the step, used when parameter ДанныеIterations User Defined Incrementations or ДанныеIterations User Defined Time Step Length is true

• ДанныеTime Initial Step: initial time increment of the step, used when parameter ДанныеIterations User Defined Incrementations or ДанныеIterations User Defined Time Step Length is true

• ДанныеTime Maximum Step - introduced in 1.0: maximum time increment of the step, used when parameter ДанныеIterations User Defined Incrementations or ДанныеIterations User Defined Time Step Length is true

• ДанныеTime Minimum Step - introduced in 1.0: minimum time increment of the step, used when parameter ДанныеIterations User Defined Incrementations or ДанныеIterations User Defined Time Step Length is true

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

Ограничения

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

Примечания

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

Scripting