FEM Geometry Preparation and Meshing/de

While most designs consist of solids, it's often highly recommended to use wires or surfaces for FEM if the structure allows for that:

• if a part is slender (long and thin) and beam-like and has a regular cross-section of one of the currently supported beam section types (rectangular, circular or pipe) then it should be analyzed using beam elements (unless there are some specific forms of loading, response or unavoidable geometry details that invalidate this assumption). Basically, one should draw a centerline (some tips on how to extract it from existing solid geometry can be found in this forum thread - in short, use Draft Wire or Draft BSpline with proper snaps and lines as supports) and apply beam section with optional rotation. There's no single rule dictating when beam elements can be used but it's often advised that the cross-section dimensions should be < 1/10 of part's length for the beam assumption to be valid.

• if a part is thin-walled (such as sheet metal parts) then it should be analyzed using shell elements (unless accurate contact results are needed or some limitations of shell elements are encountered). This is very important and often overlooked. To obtain proper accuracy of results (especially when bending is involved), one needs a few elements (at least 3-5) in the thickness direction. In the case of thin-walled parts, this usually results in large meshes (especially when tetrahedrons are used since hexahedral elements can't be generated in FreeCAD) and large computational cost - high computer power requirements and long solving time. To obtain the geometry suitable for analysis with shell elements, one should draw a midsurface of the part (some tips on how to extract it from existing solid geometry can be found in this forum thread, this one and this one - in short, apply PartDesign SubShapeBinder or Draft Facebinder, then Part Offset and finally use SubShapeBinder and Extrude to extend edges of the midsurfaces and thus close the gaps between them) and apply proper thickness. Again, there's no single rule but it's usually recommended that the thickness should be < 1/10 of a typical global dimension (length/width) for the shell assumption to be valid.

• in some cases, 2D analyses are also possible and can be enabled by setting the DatenModel Space property of the CalculiX solver:
  • plane stress - for thin parts that can be simplified to flat surfaces representing the profile for extrusion (thickness is defined in the same way as for shells), are loaded and deform only in-plane and have zero stress in the out-of-plane direction. Only two degrees of freedom are available - X and Y translation. Surfaces have to lie on the XY plane in this case. This approach is quite common. For example, a thin plate subjected to tension can be analyzed this way.
  • plane strain - for thick parts that can be simplified to flat surfaces representing the profile for extrusion (thickness is defined in the same way as for shells), are loaded and deform only in-plane and have zero strain in the out-of-plane directions. Only two degrees of freedom are available - X and Y translation. Surfaces have to lie on the XY plane in this case. This approach is not so common. For example, a long dam, wall or pipe subjected to uniform pressure at a whole length can be analyzed this way.
  • axisymmetric - for parts that can be simplified to flat surfaces representing the profile of revolution (thickness is irrelevant here) and are loaded uniformly around the whole circumference. Only two degrees of freedom are available - radial and axial translation. Surfaces have to lie on the XY plane, on the right of the Y axis. This approach is very common. For example, some pressure vessels, rubber mounts, bushings, gaskets, flanges and even bolted joints (treating the thread as axisymmetric) can be analyzed this way.

The geometry used for FEM has to be valid. Most importantly, there can't be any intersections. It's a common issue often occurring when assemblies are modeled without proper constraints between the parts. The Part SectionCut tool can help find such interferences between parts. Of course, Part Fuse may help resolve them if they are intentional. Other issues with the geometry (such as non-manifold geometries, redundant edges or faces and so on) also have to be fixed before proceeding to meshing. The Part CheckGeometry tool can be helpful but visual checks are also important. When preparing a simulation using solid elements and in doubt whether the part is really solid or just a closed shell, the aforementioned tools (Part SectionCut and Shape Content tab of the Part CheckGeometry tool output) may clarify this.

Surface meshes, typically imported from STL, OBJ and similar files or created in the Mesh Workbench, can't be used directly for FEM. It is necessary to create a shape from mesh first. Then this shape can be meshed in the FEM workbench to create a surface (shell / 2D) finite element mesh. If a solid (3D) finite element mesh is needed, shape creation has to be followed by conversion to a solid.

Designs prepared in CAD software are typically too detailed to be suitable for FEM simulations. In many cases, it's necessary to simplify them first. This step is often overlooked but it's very important because it can be hard to obtain a good mesh when the part is too detailed and even if such a mesh is obtained eventually, it might be very dense, leading to unreasonable solving times. Thus, one should always look at the design and try to simplify it as much as possible, leaving only those geometric features that may have a significant impact on the results (strength/stiffness) and thus can't be ignored. The following features are typically omitted:

• small fillets and chamfers,
• small holes,
• other small details,
• welds,
• bolts, threads,
• decorative elements (logos, engravings).

Geometry simplification for FEM may also mean cutting it in one of the symmetry planes to make use of the planar symmetry assumption in the analysis. This assumption is valid only when all the following aspects of the model exhibit symmetry in a given plane:

• geometry,
• loads,
• boundary conditions,
• response (one has to be careful with frequency/buckling analyses utilizing symmetry - antisymmetric mode shapes won't be obtained).

The use of symmetry (1/2, 1/4 or 1/8 of the model) is recommended whenever possible since it can highly reduce the computational cost of the analysis. Another advantage is that it eliminates some rigid body motions, making it easier to constrain the part. A symmetry boundary condition should be applied to the faces belonging to the plane of the cut:

• translation in the direction normal to the symmetry plane should be blocked for solid parts,
• translation in the direction normal to the symmetry plane and rotations other than around the axis normal to the symmetry plane should be blocked for shell and beam parts.

Applied force should be properly reduced if the symmetry plane cuts the region to which the force is applied (irrelevant when pressure load is used).

Another, less common type of symmetry available in FreeCAD FEM is cyclic symmetry. It can be defined using the tie constraint and makes it possible to analyze only a single representative sector of a structure consisting of such circular patterns around an axis. The assumption is that boundary conditions and loads also exhibit this form of symmetry. Tangential loads can be applied and thus torsion can be simulated this way. However, centrifugal load is commonly used with cyclic symmetry. This approach might be used e.g. for rotors, shafts, turbines, fans and flywheels.

In the case of surface (shell) geometries, the easiest way to make a sketch-based partition could be to use the Boolean Fragments tool (like for the partitions on the faces of solids). However, as explained here, when mesh group creation is enabled in the FEM preferences, it may not work properly and the following approach should be used:

1. Create a face for one side using e.g. the Part MakeFace tool (e.g. a square plate with a circular hole).
2. Create a face for the other side in an equivalent way (e.g. a circular face filling the hole in the square plate).
3. Apply the Part Builder tool with the Shell from faces mode and disabled Refine shape checkbox to the previously created faces.

Partitioning only the selected faces of a solid using datum planes instead of sketches without splitting the whole volume is also tricky. One possible approach is to:

1. Downgrade the body to faces.
2. Select that one face and datum plane and use the Slice apart tool.
3. Delete the Exploded Slice container without deleting its contents.
4. Select all faces and slices and Upgrade them to Shell.
5. Upgrade the Shell to Solid or use the Convert to solid tool.

Another way is to:

1. Create a subshapebinder of the face to be partitioned.
2. Split the subshapebinder with the datum plane using the Slice apart tool.
3. Create a new Body (to avoid cyclic dependency).
4. Create a new subshapebinder from the edges obtained from the intersection of the previous subshapebinder and datum plane.
5. Select the original Body and the new subshapebinder and use the Boolean fragments tool.

Other ideas can be found in this forum thread but they are more case-specific.

One of the current major limitations of the FEM workbench is that multiple meshes are not supported. In practice, this means that one cannot mesh each part of the assembly individually and then connect the parts with proper constraints for the analysis. Instead, it's necessary to create a single object containing all the parts of the assembly and mesh it. There are several different options here, all relying on Part boolean tools. The choice depends on the desired effect - whether the individual parts/volumes and their boundaries should be selectable (e.g. for material assignments or definitions of boundary conditions acting on internal faces) or not:

• Part Fuse - merges the parts, making it impossible to select them individually e.g. for material definitions,
• Part Compound - creates a compound object, making it possible to select individual parts,
• Part JoinConnect - works like Part Fuse, merges the parts, making it impossible to select them individually,
• Part BooleanFragments - works like Part Compound, making it possible to select individual parts.

It's important to mention that if the parts are exactly touching, a continuous mesh will be created on the boolean object and no constraints will be needed for the simulation (unless Part Compound is used and nodes aren't coincident or Gmsh's Coherence Mesh property is set to false). If there's even a small gap (or an intersection within a Part Compound) between the parts, the mesh won't be continuous and constraints like tie or contact will be needed. Running a frequency analysis is a good way to reveal if the mesh is continuous or not - if the parts are not connected, the first mode shapes with deformation visualized using Warp filter will show separation - the parts will "fly away".

It is often advised to use Boolean fragments with Compsolid mode and then apply a Compound filter to it, particularly when analyzing multi-material assemblies and solids embedded in other solids without cutouts (like in the FEM Shear of a Composite Block tutorial). As can be seen in the Shape Content tab of the Check geometry tool (it is important to use this tool when in doubt in such cases), Compound filter removes the Compound and leaves only the Compsolid consisting of multiple solids connected by their faces.

Selection of internal regions (e.g. faces/volumes) can be tricky. It might be needed for the application of different materials, body loads or boundary conditions (especially in thermal and electromagnetic analyses). Several ways are possible:

• enabling clipping plane for the time of selection and picking internal faces,
• hiding the boolean object, showing only one of the parts it was applied to and selecting it,
• enabling transparency and using the Selection view with the Picked object list option checked as described here,
• selecting another, external object and editing the References property on the Data tab of a given analysis feature (requires manual specification of the geometric object's number).

Too coarse mesh is one of the most common sources of inaccuracies and other issues in FEM. It's often a partial fault of automatic mesher settings - they typically generate very coarse, unsuitable meshes when the element size is not manually specified but left with a default value. One should always know the approximate dimensions of the part, especially the size of the smallest relevant feature (Std Measure tool can be used to find it) and specify the proper maximum element size based on that. There is also a minimum element size setting that can prevent the creation of too tiny elements around small geometric features which may lead to unnecessarily dense meshes (and sometimes even FreeCAD crashing or freezing when trying to generate such meshes). Generally speaking, it's better to start with a coarser mesh (taking less time to generate), see what it looks like (some experience is necessary) and refine it if necessary. It often makes sense to use dense mesh only around the areas of interest (locations with large stress gradients/concentrations - notches) and relatively coarse mesh away from them. This way, the number of elements can be significantly reduced, leading to shorter solving times. Local mesh refinement is defined using FEM MeshRegion.

If the above rules are followed (especially regarding geometry validity, defeaturing and element size selection), the mesh should be generated correctly. However, in some cases, the geometry can't be simplified too much, or the modeling procedure is appropriate but leads to small edges and faces anyway. Then meshing with second-order elements may fail due to negative Jacobians. The reason is that meshers have to follow the CAD model and put the mid-side nodes of second-order elements on the geometry. With more complex shapes, it may lead to elements being stretched so much that they become inverted. Jacobian is one of the most common mesh quality measures. It represents the element's deviation from the ideal shape. It becomes negative when the element turns inside out (becomes inverted) either due to large deformation during the analysis (not considered here) or because of the aforementioned meshing issues. Negative Jacobians in FreeCAD FEM might be reported by Gmsh or by CalculiX. Their locations in the mesh are highlighted when CalculiX analyses are submitted using the Run solver calculations button. The following tips can help eliminate them:

• set the Second Order Linear property of the FEMMeshGmsh object to true - this results in the mid-side nodes of second-order elements being just added in the middle of straight (initially) first-order element edges, without snapping them to the geometry and resolves the issue in most cases,
• use Netgen instead of Gmsh - Netgen is known to be less prone to negative Jacobian issues but also doesn't report them so the user may find out only when submitting the analysis,
• further reduce the element size,
• export the geometry, try meshing it in Gmsh or Netgen (NGSolve) GUI or other standalone mesher (like Salome_Meca) - those tools have additional features that can help get rid of negative Jacobians (for example, Gmsh has so-called "High-order tools"),
• use first-order elements - should be done only as a last resort since first-order tetrahedrons are known for their inaccuracy.

Mesh convergence studies are recommended in all serious projects requiring accurate results. The reason is that the results can change a lot, approaching correct values when the mesh is refined. The following approach should be used:

1. After obtaining the first results and noting them (usually maximum von Mises stress, von Mises stress at a given location and maximum displacement), refine the mesh (globally or better locally - with FEM MeshRegion) and rerun the simulation.
2. Check the results and note their new values. If they differ significantly from the initial results, refine the mesh further and rerun the analysis.
3. Repeat the process if the results still change (usually grow) significantly with mesh refinement.

It usually helps to create a plot with a given result vs mesh density. This way it's easier to notice when the results start to converge. The acceptable difference in results between two runs is usually around a few percent (e.g. below 5%).

In some cases, it may happen that the maximum stress will be growing indefinitely regardless of how dense the mesh will be. Such a non-physical effect is known as a stress singularity. It may occur due to the following reasons:

• concentrated forces applied to solid and shell models,
• boundary conditions applied to points (individual nodes),
• sharp corners,
• contact occurring at a corner.

Typical ways of dealing with stress singularities are:

• applying loads and boundary conditions to small areas instead of points - see the section about partitioning above,
• adding small fillets to sharp corners (an exception to the rule of omitting small fillets when simplifying the geometry for FEM),
• including plasticity in material behavior to enable stress redistribution and limit the stresses to values allowed by the plasticity definition while observing the proper level of yielding (plastic strain),
• ignoring singularities and reading stresses away from them if possible (based on St. Venant’s Principle).

Typical mesh convergence plots:
- displacement (green curve) converges quickly,
- maximum stress at a notch like a hole (blue curve) needs more iterations of mesh refinement to converge,
- maximum stress at a sharp corner with a fixed boundary condition (red curve) doesn't converge at all. Stress singularity occurs and a small fillet would have to be added and the connection would have to be modeled in more realistic, flexible way to avoid this behavior.