1. Model Creation Summary¶
This section summarizes the steps involved in creating a finite element knee model. The summary includes links to other chapters where specific details are provided. This chapter also describes the inputs and outputs of each step.
These steps apply to the DU data set. The documentaiton for the OpenKnee(s) data set can be found in a separate document.
Additionally, ligaments and tendons are modeled as bundles of springs, however the steps for modeling these tissues as a continuum are also documented. This additional documentation is included to prevent excessive use of revisions if it is decided to represent ligaments and/or tendons as a continuum.
1.1. Image Segmentation and Reconstruction¶
The MR images are used to define two types of data
- Label maps
- Insertion sites (for spring representation)
Label maps are used to represent 3D geometry, and that geometry is reconstructed into surfaces. The insertion sites are used to define ligament and tendon geometry that are modeled as bundles of springs. The ligaments and tendons that are modeled as bundles of springs do not need label maps or surface models.
The segmentation process is described in the image segmentation section, and the reconstruction process is described in the geometric reconstruction section. The process used to define ligament and tendon insertion sites and geometry are described in the ligament and tendon meshing section.
Ligaments and tendons are modeld as bundles of springs. One spring is defined by connecting one insertion point to another. Multiple springs are used to represent a ligament, and these springs are linearly distributed across the insertion area. To achieve this, the user places two points at the margins of each insertion area (4 total for each ligament/tendon). The insertion areas as identified using literature descriptions of soft tissue anatomy. The specific details on how this process are described in the ligament and tendon meshing section.
If in the future, a ligament and/or tendon is being modeled as a continuum, then the geometry should be segmented and reconstructed like the other geometry.
1.1.1. Segmentation Inputs¶
- MR images
- The CT images supplied with the DU data set are not used.
1.1.2. Segmentation Outputs¶
The outputs of segmentation are label maps that are defined from the MR images.
- Label maps
- Femur
- Tibia
- Patella
- Femur cartilage
- Tibia cartilage
- Patella cartilage
- Medial meniscus
- Lateral meniscus
- Insertion sites for ligament/tendon spring model (4 points defined with respect to the MR image coordinate system)
- Ligaments
- Tendons
1.1.3. Reconstruction Inputs¶
The label maps that are output from segmentation are the inputs for geometric reconstruction. These inputs are the label maps for the femur, tibia, patella, cartilage, and medial and lateral meniscus. Ligaments and tendons are modeled as bundles of springs, therefore they do not have label maps, and they are not reconstructed into surfaces.
If in the future, a ligament and/or tendon is being modeled as a continuum, then ligament/tendon label maps created during segmentation should be reconstructed into surfaces.
1.1.4. Reconstruction Outputs¶
Geometric reconstruction uses the label maps to define surfaces. One surface is created for each label map, and these surfaces are saved as .stl files.
- Femur surface .stl
- Tibia surface .stl
- Patella surface .stl
- Femur cartilage surface .stl
- Medial tibial cartilage surface .stl
- Lateral tibial cartilage surface .stl
- Patella cartilage surface .stl
- Medial meniscus surface .stl
- Lateral meniscus surface .stl
1.2. Mesh Creation¶
The surfaces that were created during the Image Segmentation and Reconstruction are used to create the solid meshes that are used in the finite element model. The bones and cartilage are modeled as rigid bodies, so the surfaces created for the femur, tibia, and patella are used as the finite element meshes for those geometries. The cartilage is being modeled using an elastic foundation model ([LKST15],:cite:halloran_comparison_2005), so the meshes for the femoral cartilage, tibial cartilage (medial and lateral) and the patellar cartilage are being converted into quadrilateral dominated surfaces. The menisci are modeled as solids, and the surfaces are used to create hexahedral meshes, and the hexahedral meshes are used in the finite element model. If in the future, a ligament and/or tendon is being modeled as a continuum, then the geometry should also be meshed using hexahedral elements following the same procedure as used for meshing the menisci.
Specific details on the meshing process are described in the meniscus meshing and cartilage meshing sections.
The insertion points for the ligaments and tendons are used to define the individual fibers that connect the insertion sites. The insertion sites are used to define the initial ligament and tendon geometry. See the ligament and tendon meshing section for more details on ligament and tendon mesh creation.
Note that the number of elements used in the ligament, cartilage, and menisci geometry will be determined with convergence studies.
1.2.1. Meshing Inputs¶
- Solid Geometry
- Medial meniscus surface (.stl)
- Lateral meniscus surface (.stl)
- Elastic Foundation Geometry
- Femur cartilage surface (.stl)
- Medial tibial cartilage surface (.stl)
- Lateral tibial cartilage surface (.stl)
- Rigid Geometry
- Femur surface (.stl)
- Tibia surface (.stl)
- Patella surface (.stl)
- Ligament and Tendon Geometry
- Insertion sites (4 points defined with respect to the MR image coordinate system)
- Desired number of fibers for each ligament and tendon
- Desired number of “cross elements” for each ligament and tendon (see ligament and tendon meshing for more information)
1.2.2. Meshing Outputs¶
- Solid Geometry
- Medial meniscus hexahedral mesh (abaqus .inp file)
- Lateral meniscus hexahedral mesh (abaqus .inp file)
- Elastic Foundation Geometry (rigid)
- Femur cartilage quadrilateral dominated mesh (abaqus .inp file)
- Medial tibial cartilage quadrilateral dominated mesh (abaqus .inp file)
- Lateral tibial cartilage quadrilateral dominated mesh (abaqus .inp file)
- Patellar cartilage quadrilateral dominated mesh (abaqus .inp file)
- Rigid Geometry
- Femur triangular surface mesh (abaqus .inp file)
- Tibia triangular surface mesh (abaqus .inp file)
- Patella triangular surface mesh (abaqus .inp file)
- Initial Ligament and Tendon Geometry
- Ligament spring mesh (abaqus .inp file, one file for each ligament)
- Tendon spring mesh (abaqus .inp file, one file for each tendon)
1.3. Reference Simulation¶
The initial ligament and tendon meshes are defined by connecting insertion points with straight lines, and they may overclose the bones, cartilage, and menisci. A reference simulation is used to make the ligaments and tendons wrap around any bodies that they may initially overclose. The purpose of the reference simulation is to modify the node positions of the initial ligament and tendon meshes to account for wrapping. The reference state mesh and reference simulation boundary conditions sections describes this process in more detail.

Fig. 1.1 An example of (a) the initial mesh that is defined from insertion point to insertion point data, and (b) the reference state where the ligament’s mesh wrapped around the femur and tibia surfaces. Note that this is used as an example, and not used to describe the insertion locations or size of any specific ligament.
1.3.1. Reference Simulation Inputs¶
- Solid Geometry
- Medial meniscus hexahedral mesh (abaqus .inp file)
- Lateral meniscus hexahedral mesh (abaqus .inp file)
- Rigid Geometry
- Femur cartilage mesh (abaqus .inp file)
- Medial tibial cartilage mesh (abaqus .inp file)
- Lateral tibial cartilage mesh (abaqus .inp file)
- Femur triangular surface mesh (abaqus .inp file)
- Tibia triangular surface mesh (abaqus .inp file)
- Patella triangular surface mesh (abaqus .inp file)
- Initial Ligament and Tendon Geometry
- Ligament spring mesh (abaqus .inp file, one file for each ligament)
- Tendon spring mesh (abaqus .inp file, one file for each tendon)
1.3.2. Reference Simulation Outputs¶
- Updated Ligament and Tendon Geometry (new node positions)
- Ligament spring mesh (abaqus .inp file, one file for each ligament)
- Tendon spring mesh (abaqus .inp file, one file for each tendon)
1.4. Coordinate Systems¶
The rigid body coordinate systems are defined for the femur, tibia, and patella. Specific details on those processes can be found in the coordinate systems section.
These rigid body coordinate systems are used to define connector elements, and the nodes that compose the connector elements. These elements are used to assign boundary conditions and/or loads to the joint coordinate system, and to also measure joint motion with respect to the joint coordinate system. The specific information on connector element definition can be found in the connector elements section.
1.4.1. Coordinate Systems Inputs¶
- User selected points from MR images (used for initialization)
- Femoral landmarks
- Tibial landmarks
- Patellar landmarks
- Digitized points
- Femur
- Femoral articulating surface
- Femoral landmarks
- Tibia
- Tibia articulating surface
- Tibial landmarks
- Patella
- Patella articulating surface
- Patellar landmarks
- Surfaces (.stl)
- Femur
- Femoral cartilage
- Tibia
- Tibial cartilage
- Patella
- Patellar cartilage
1.4.2. Coordinate Systems Outputs¶
- Connector element definitions (abaqus .inp file)
1.5. Interactions and Ties¶
Rigid ties are used to simulate insertions of the ligament, tendons, and meniscal attachments. Similarly, the cartilage is rigidly tied to the corresponding bone. Interactions are used to define contact between different bodies.
This section does not have specific inputs or outputs. The ties and interactions are described in the interactions and ties section, and the sequence with interactions are activated are described in the simulation steps section.
1.6. Simulation Steps and Boundary Conditions¶
The different steps used in a FEA simulation, and boundary conditions are described in the simulation steps and boundary conditions section.
In general, the passive flexion simulation starts with applying a nominal 20 N load to the quadricep along the quadricep’s line of action, while the femur and tibia are fixed. This is followed by the femur being flexed from it’s initial position to 0 degrees flexion. The 20 N quadricep load is maintained, and a 20 N compressive load is also applied to the femur throughout this step.
The last step in the passive flexion simulation flexes the femur about it’s medial-lateral axis from 0 to 90 degrees. There is a nominal 20 N compressive load applied to the joint to maintain joint contact. Similarly, there is a nominal 20 N load applied to the quadricep to maintain contact between the femur and the patella.
1.7. Model Outputs¶
The model outputs are measured from the finite element simulation results. Custom Python scrits are used to read/extract the desired results from the simulation’s results file. The outputs are described in the Model Outputs section.
The main output variables are:
- Contact (area, force, and pressure)
- Joint kinematics
- Ligament forces