5.3 Editing Geometry¶

The Edit panel, one of the panels on the Build panel, gives access to the object's creation parameters and editing options.

The other feature to note at the top of both the Edit and Mesh panels is the Object rollout. This shows the name of the active object as well as its type. The type of the object affects what tools will be available for editing and meshing the geometry.

An object can be converted to a different type via the Convert button. Two options are available:

Editable surface: An object of this type will have a surface mesh that can be modified. A separate volume mesh can be generated for this object.
Editable mesh: An object of this type will only contain a volume mesh and this mesh can be modified if necessary.

Editable surfaces and editable meshes will be explained in detail in section Creating and Editing a Mesh.

Editing Primitives¶

For primitives the same parameters as when the object was created are shown on the Edit panel. This allows you to change the primitives dimensions at any time. If the object is not a primitive, no options will be shown here.

Note that changing the primitive parameters will discard the FE mesh if one was already created. The primitive will have to be meshed again.

Editing Editable Surfaces¶

An editable surface is defined via a surface mesh. This surface mesh can be modified via the tools on the Edit panel.

Note that changing the surface mesh of an editable surface will discard the FE mesh if one was already created. The object will have to be meshed again.

The sections below discuss each of the available tools in more detail.

Auto Partition¶

The surface of an editable surface can be partitioned (i.e. divided) into several partitions. By default, FEBio Studio will automatically generate a partitioning based on finding the crease edges. If for some reason the resulting partitioning is not correct, the user can re-run the auto-partitioning tool.

The auto-partition tool partitions the geometry into surfaces by identifying the crease edges. A crease edge is an edge between two surface facets whose normals make an angle that is larger than the crease angle. To manually create surface partitions, use the Partition tool instead.

Decimate¶

Decimation is the process of decreasing the number of triangles in the mesh. This tool decimates the triangular surface mesh using an approximate Centroidal Voronoi Diagram based approach.

Scale: This option helps in creating a uniform triangular mesh. Scale value specifies the desired reduction in the total number of nodes in the final decimated mesh. For example a 0.4 value of scale will result in the final decimated mesh with 40% of current number of nodes.

Edge Collapse¶

This filter collapses all edges with a length that is below the given threshold value. This can be useful for eliminating small triangles or very narrow triangles, which may improve the quality of the mesh.

Fix Mesh¶

This tool provides several options to fix specific common problems in surface meshes.

Remove duplicate elements: removes elements that are repeated in the mesh.
Remove non-manifold elements: removes element that have an invalid connectivity.
Fix winding: This option works only for triangular mesh. This option checks if the nodes of the triangle are in the same sequence clockwise/anti-clockwise direction for all the triangular facets.
Fill all holes: Finds and fills the holes in the triangular mesh by adding new triangular faces.

Flip Edges¶

Flips the selected edge. This can be useful to eliminate slivers or otherwise locally improve the mesh quality.

MMG Remesh¶

The MMG Remesh tool uses the MMG library¹ to regenerate the surface mesh. The following options can be set.

Element size: Desired element size.
Min element size: The minimum element size allowed. MMG cannot always guarantee that this criterion is met.
Global Hausdorff value: Sets the maximum allowed distance from the triangle mesh to the locally interpolated quadratic surface. Setting this to a smaller value creates a refined mesh in areas of large curvature. Note that this is a distance, so the units are length.
Gradation: Sets the rate of transition between a refined and coarser area. A value close to one creates a very wide transition area. Larger values allow for narrower transition areas.
Only remesh selection: If checked (and a current selection is active), only the selection will be remeshed.

This tool can be used for globally remeshing the surface, or for doing a local mesh refinement. To perform a local mesh refinement, select the faces that should be refined, and make sure to check the “only remesh selection” option.

Partition¶

The Partition tool creates a partition (i.e. a selectable geometry surface) from the current node, edge, or face selection.

This tool is useful when the auto-partition tool did not create a desirable partitioning of the surface mesh.

Project Curve¶

This tool projects a curve on the mesh and modifies the mesh locally so that the curve becomes a crease edge of the surface mesh.

First, select the curves (i.e. edges of other geometry) and assign them to the selection box. Then, click Apply.

Refine¶

This tool uniformly refines the mesh by splitting all elements. Triangles are split into 3 triangles, and quads are split into 3 smaller quads.

Smooth¶

Performs a simple mesh smoothing, where each node is moved towards the average of its neighbors. The new node position is defined by,

\[ \boldsymbol{r}_{new}=(1-\lambda)\boldsymbol{r}_{old}+\lambda\boldsymbol{r}_{c} \]

Here, \(\boldsymbol{r}_{new}\)is the new position, \(\boldsymbol{r}_{old}\)is the old position, \(\boldsymbol{r}_{c}\)is the average of the node neighbors, and \(\lambda\) is a weight factor.

The following parameters can be set:

Iterations: Enter the value to repeat the smoothing operation several times.
lambda: The weight factor \(\lambda\) in the equation above.
preserve shape: When checked, the new nodal positions are projected back onto the original mesh. This is useful the counteract the shrinking that typically occurs when applying this smoothing filter.
preserve edge: When checked, nodes that were on an edge on the original geometry, are forced to remain on that edge.

Weld Nodes¶

The Weld Nodes tool merges the selected nodes that are within the specified tolerance. Any edges or faces that collapse as a result, will be removed from the mesh as well.

https://www.mmgtools.org/ ↩