When using FreeCAD 0.17 it is not that difficult to make a simulation of something pressuring a cube that is fixed to the ground. I’t a simple case where we follow the typical simulation procedure… Make drawing, define boundary conditions, generate mesh, solve and get results.

I can understand that I need boundary conditions since these are the essence of the problem. But the mesh seems out of place. Or not… It is the building block of the finite element method where we describe a complex geometry into multiple small connected elements. The mesher will transform the solid in building blocks that represent the geometry we wish to study. We can use a mirrad of element types (block shapes) and the mathematical formulations they hold. NetGen should not be any different it can have tetrahedrons, hexahedrons, … and each specific nodes required…

But a question which came to my mind was how would the element shape originator and the element formulation originator work. Are they the same?Why I make this question? In freeCAD I generate a mesh with NetGen or Gmsh, however I solve it with Calculix and not the solver from NGSolve or Gmsh.

Before attempting a solution, a mesh is generated and thus the shape of the elements is defined and from the images they look tetrahedrons.

I found an answer to my questions in a paper written by one of the Authors of NetGen: Joachim Schöberl: An advancing front 2D/3D-mesh generator based on abstract rules.

The mesh is generated according to a specific sequence from a geometry. First special points are gathered on the corners of the target geometry, next edges have to be detected to then create a surface mesh that follows specific element shape rules; the final step is to create a volume mesh from the surface mesh and another specific rules necessary for element quality.

The output should be a cloud of nodes, elements and their connectivity to each other. From the paper it looks like it is purely connected to the geometry but then what connects to the differential equations we wish to solve? For instance how do I say a line is a beam? Or how do I create a body shell which basically is a shell with thickness.

Here comes the solver part. In case of calculix with NetGen used in this example all tetrahedrons should have a specific element type which will define the physics involved being structural, thermal, electric. In this case structural.

Indirectly the program gives a hint of the element type suggesting structural loads and forces in the boundary conditions or for a thermal case (not this one), the appropriate thermal boundary conditions.

As an example I am picking a Cube made in FreeCAD using NetGen mesher and Calculix solver. Before entering the solving process I generated the .inp file which contains the mesh, the boundary conditions and the material data to perform the simulation.

Somewhere in the .inp file you will find the following:

TYPE=C3D10

The element type name used is C3D10, as expected expected since normally the solver has a ton of element types, and there should also be in the Calculix solver a similar variety like for instance Ansys with Solid187 (https://www.sharcnet.ca/Software/Ansys/17.0/en-us/help/ans_elem/Hlp_E_SOLID187.html), Solid186 or Solid226; for a list see this reference:

https://www.sharcnet.ca/Software/Ansys/17.0/en-us/help/ans_elem/

More details about C3D10 element can be seen in:

http://web.mit.edu/calculix_v2.7/CalculiX/ccx_2.7/doc/ccx/node33.html

And a list off all Calculix elements can be seen here:

http://web.mit.edu/calculix_v2.7/CalculiX/ccx_2.7/doc/ccx/node25.html

** written by FreeCAD inp file writer for CalculiX,Abaqus meshes ** Nodes *Node, NSET=Nall 1, 10, 10, 0 2, 10, 10, 10 3, 10, 0, 0 4, 10, 0, 10 5, 0, 10, 0 6, 0, 10, 10 7, 0, 0, 0 8, 0, 0, 10 9, 0, 5, 10 10, 5, 10, 10 11, 10, 5, 10 12, 5, 0, 10 13, 0, 5, 0 14, 5, 10, 0 15, 10, 5, 0 16, 5, 0, 0 17, 10, 10, 5 18, 0, 10, 5 19, 10, 0, 5 20, 0, 0, 5 21, 5, 5, 10 22, 5, 5, 0 23, 5, 10, 5 24, 5, 0, 5 25, 10, 5, 5 26, 0, 5, 5 ** Volume elements <span style="color: #0000ff;"><strong>*Element, TYPE=C3D10, ELSET=Evolumes</strong></span> 25, 7, 4, 6, 8, 24, 21, 26, 20, 12, 9 26, 7, 6, 4, 1, 26, 21, 24, 22, 23, 25 27, 5, 7, 1, 6, 13, 22, 14, 18, 26, 23 28, 4, 7, 1, 3, 24, 22, 25, 19, 16, 15 29, 4, 2, 1, 6, 11, 17, 25, 21, 10, 23 ** Define element set Eall *ELSET, ELSET=Eall Evolumes *********************************************************** ** Element sets for materials and FEM element type (solid, shell, beam, fluid) ** written by write_element_sets_material_and_femelement_type function *ELSET,ELSET=SolidMaterialSolid Evolumes *********************************************************** ** Node sets for fixed constraint ** written by write_node_sets_constraints_fixed function ** FemConstraintFixed *NSET,NSET=FemConstraintFixed 3, 4, 7, 8, 12, 16, 19, 20, 24, *********************************************************** ** Materials ** written by write_materials function ** Young's modulus unit is MPa = N/mm2 ** FreeCAD material name: 1C60 ** SolidMaterial *MATERIAL, NAME=SolidMaterial *ELASTIC 210000, 0.300 *********************************************************** ** Sections ** written by write_femelementsets function *SOLID SECTION, ELSET=SolidMaterialSolid, MATERIAL=SolidMaterial *********************************************************** ** At least one step is needed to run an CalculiX analysis of FreeCAD ** written by write_step_begin function *STEP *STATIC *********************************************************** ** Fixed Constraints ** written by write_constraints_fixed function ** FemConstraintFixed *BOUNDARY FemConstraintFixed,1 FemConstraintFixed,2 FemConstraintFixed,3 *********************************************************** ** Node loads Constraints ** written by write_constraints_force function *CLOAD ** FemConstraintForce ** node loads on shape: Box:Face4 1,2,-0.0000000000000E+00 2,2,-0.0000000000000E+00 5,2,-0.0000000000000E+00 6,2,-0.0000000000000E+00 10,2,-1.6666666666667E+02 14,2,-1.6666666666667E+02 17,2,-1.6666666666667E+02 18,2,-1.6666666666667E+02 23,2,-3.3333333333333E+02 *********************************************************** ** Outputs --&gt; frd file ** written by write_outputs_types function *NODE FILE U *EL FILE S, E ** outputs --&gt; dat file *NODE PRINT , NSET=Nall U *EL PRINT , ELSET=Eall S *********************************************************** ** written by write_step_end function *END STEP *********************************************************** ** CalculiX Input file ** written by write_footer function ** written by --&gt; FreeCAD 0.17.12321 (Git) ** written on --&gt; Sun Oct 8 21:43:43 2017 ** file name --&gt; ** analysis name --&gt; Analysis ** ** ** ** Units ** ** Geometry (mesh data) --&gt; mm ** Materials (Young's modulus) --&gt; N/mm2 = MPa ** Loads (nodal loads) --&gt; N **