FEM Geometry Preparation and Meshing/zh-hans

Geometry validity

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 normals

In case of surface geometries used for analyses with shell and 2D elements, the normal directions of the surfaces might be important. They are used to distinguish the positive and negative side of a surface finite element mesh and affect analysis features such as pressure loads and contact. Moreover, 2D analyses (plane stress/strain and axisymmetric) with CalculiX require the normals to point in the positive Z direction. If they are inverted, negative jacobian errors will occur.

To check the normals, use one of the following approaches:

• enable Backlight in the Preferences and set the ViewLighting property of the surface object to One side - the negative normal direction will appear darker,
• use the Normal Vector macro,
• mesh the surface shape in FEM - the mesh will be colored only on the positive normal side.

To invert the normals, use the Reverse shapes tool.

Using surface meshes for FEM

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.

The biggest issue with shapes created from surface meshes is that all their triangles become the faces of the generated shape. In FEM, this makes the assignment of analysis features (such as loads and boundary conditions) particularly problematic. In the case of planar surfaces, refinement after conversion to a solid may remove the redundant triangular faces. In practical scenarios, most will remain though and because of that, surface meshes are not recommended for use in FEM. CAD geometries (created in FreeCAD or imported from STEP/IGES files) should be used instead. Sometimes it may even make sense to recreate the geometry based on the surface mesh.

Geometry simplification

Defeaturing

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).

The Part Defeaturing tool and add-on Defeaturing Workbench can be helpful when simplifying parts for simulations.

Original bracket geometry

Bracket geometry simplified using only the Part Defeaturing tool

Replacing parts with boundary conditions

In the case of assemblies (more about them in one of the next sections), often some parts can be excluded from simulations and replaced with boundary conditions if they were attached to parts being analyzed. Such approach is valid if the excluded parts are significantly stiffer (in terms of structural stiffness so considering not only elasticity of the material but also geometry of the part) than the analyzed parts to which they were connected. That's because fixed boundary conditions introduce rigidity (as if the analyzed part was attached to an infinitely stiff component) and flexible supports like spring elements are not available in the FEM workbench of FreeCAD when using CalculiX (Elmer has FEM ConstraintSpring).

Model of 1/8 of a cylindrical pressure vessel with symmetry boundary conditions and internal pressure load

Utilizing cyclic symmetry

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.

Geometry partitioning

Partitioning basics

So-called partitioning is a division of the geometry into smaller segments. In other software, it's commonly used to allow hex meshing, but in FreeCAD it can be useful for other reasons too:

• creating subregions for analysis feature assignments,
• splitting parts into sections made of different materials,
• creating regions for mesh refinement,
• controlling the meshing algorithm by forcing it to follow additional edges (particularly useful to control Gmsh's mesh growth).

Partitioning faces of solids with sketches

The main application of partitioning is when a load (or a boundary condition) has to be applied only to a selected region of the part's surface. The easiest way to achieve it for solid parts is to create a sketch with a proper contour on that face and use the Part Boolean Fragments tool to split the face with the sketch.

Part with a face partition for load or boundary condition application

Partitioning volumes of solids with datum planes

Another reason for partitioning is when multiple materials have to be applied to a single part (without having to use multiple parts connected with each other). Then, partitioning can be done using a datum plane and Part Boolean Fragments tool with the Compsolid mode.

Partitioning surface geometries with sketches

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.

Square plate with a circular face partition

Partitioning faces of solids with datum planes

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.

Cylindrical face of a hole partitioned with a plane to apply 180° load from a pin

Assembly geometries

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 / Netgen's Glue 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".

The first mode shape of a frequency analysis visualized with the Warp filter - two cubes with a small initial gap were analyzed

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), the Compound filter removes the Compound and leaves only the Compsolid consisting of multiple solids connected by their faces. This approach is recommended because a compound is just a container with topologically unconnected shapes and may include all kinds of shapes, so the mesher may not be able to use it properly (mesh just the solids as the user wishes). Operations such as Boolean fragments always create Compounds, and the Compound filter is used to extract the relevant shape out of the Compound. When using this approach, even tiny gaps/misalignments should still be avoided. Otherwise, it might be necessary to use non-default Compound filter settings as shown in this forum thread.

Workarounds for errors such as:

and:

include:

• leaving the last material without any solid assigned (it will be automatically assigned to all solids that aren't referenced in other material definitions),
• using Netgen instead of Gmsh to create the mesh,
• separating the parts a bit and applying tie constraints to connect them in the simulation.

Such errors are caused by missing or overlapping material definitions in some elements. This forum post lists references that show it in a clear way and the whole thread can be helpful in the case of similar issues as well.

Selection of interior entities

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 with cores/inclusions or external fluid domains). Several ways are possible:

• introduced in 1.1: using the Clarify Selection tool - currently the easiest method,
• 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 name and number - make sure the line corresponding to this object is still highlighted and no other unwanted objects are highlighted after entering the name with the number and click on it if it's not highlighted before confirming with OK).

Manually editing the References property

introduced in 1.1: If the selected face of CompSolid (Boolean fragments with CompSolid mode + Compound filter standard workflow described in the Assembly geometries section) belongs to two solids, a pop-up menu appears, allowing the selection of the proper solid.

Meshing basics

Choosing element size

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.

Default, too coarse mesh

Globally refined mesh

Locally refined mesh

Choosing element type

The choice of element type is not easy and depends on many factors but the general rule is that hexahedral and quadrilateral elements are preferable over tetrahedral and triangular ones. However, complex geometries can't be meshed with hexahedral elements and FreeCAD has very limited capabilities of their generation (see the Hex meshes section below). However, meshes with hexahedral elements can be imported from external meshers such as Gmsh and used in the FEM workbench as shown in this video.

Choosing element order

The choice of element order (first or second) depends on the analysis conditions but in most cases, second-order elements are preferred. This is particularly the case with triangular and tetrahedral elements - their first-order (linear) versions are normally not recommended for regular usage and they should be used only as filler elements in regions of low importance. However, since FreeCAD can't properly generate hexahedral elements, linear tetrahedrons can be used in some cases, if the meshes are dense enough. Especially when performing analyses with contact.

Quad and hex meshes

Quad meshes

Quadrilateral elements can be generated on surface geometries using both meshers:

• Gmsh - set the DataAlgorithm 2D property to Quasi-structured Quad (currently, it doesn't work for 2nd order elements) or enable the DataRecombine All property and select the DataRecombination Algorithm,
• Netgen - enable the DataQuad Dominated property.

Quad-dominated mesh generated with Netgen

Hex meshes

Hexahedral meshes can be generated on volume geometries using both meshers with some significant limitations:

• Gmsh - set the DataSubdivision Algorithm to All Hexahedra - however, the resulting elements are not shaped as expected from hexahedral meshes used in practice,
• Netgen - introduced in 1.1: for simple extruded shapes, hex or hex-dominated meshes can be created by extrusion if the DataQuad Dominated property is enabled and the DataZRefine property is set to Regular (Custom requires specifying the height of each element in the extrusion direction). The extrusion direction can be changed from the default Z using the DataZRefine Direction property. Element height can be specified as a fraction of the total height using the DataZRefine Size property. This approach works only for first-order meshes (unless the generated elements are all hexahedrons).

Hex-dominated mesh generated with Netgen's ZRefine algorithm

Negative Jacobians

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 or FEMMeshNetgen 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.

Regardless of those tips, it's important to emphasize once again that negative Jacobians are usually the fault of messy modeling approaches and lack of geometry preparation for analysis (especially common with STEP models downloaded from various websites). Even if the mesh is eventually generated in such cases, the results are likely to be of poor quality (recall the GIGO rule mentioned in the first paragraph). Thus, geometry clean-up and preparation for FEM should always be the priority.

Mesh convergence studies

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.