A Finite Element Approach for Locating the Center of Resistance of Maxillary Teeth

Summary

This study outlines the necessary tools for utilizing low-dose three-dimensional cone beam-based patient images of the maxilla and maxillary teeth to obtain finite element models. These patient models are then used to accurately locate the C_RES of all the maxillary teeth.

Abstract

The center of resistance (C_RES) is regarded as the fundamental reference point for predictable tooth movement. The methods used to estimate the C_RES of teeth range from traditional radiographic and physical measurements to in vitro analysis on models or cadaver specimens. Techniques involving finite element analysis of high-dose micro-CT scans of models and single teeth have shown a lot of promise, but little has been done with newer, low-dose, and low resolution cone beam computed tomography (CBCT) images. Also, the C_RES for only a few select teeth (i.e., maxillary central incisor, canine, and first molar) have been described; the rest have been largely ignored. There is also a need to describe the methodology of determining the C_RES in detail, so that it becomes easy to replicate and build upon.

This study used routine CBCT patient images for developing tools and a workflow to obtain finite element models for locating the C_RES of maxillary teeth. The CBCT volume images were manipulated to extract three-dimensional (3D) biological structures relevant in determining the C_RES of the maxillary teeth by segmentation. The segmented objects were cleaned and converted into a virtual mesh made up tetrahedral (tet4) triangles having a maximum edge length of 1 mm with 3matic software. The models were further converted into a solid volumetric mesh of tetrahedrons with a maximum edge length of 1 mm for use in finite element analysis. The engineering software, Abaqus, was used to preprocess the models to create an assembly and set material properties, interaction conditions, boundary conditions, and load applications. The loads, when analyzed, simulated the stresses and strains on the system, aiding in locating the C_RES. This study is the first step in accurate prediction of tooth movement.

Introduction

The center of resistance (C_RES) of a tooth or segment of teeth is analogous to the center of mass of a free body. It is a term borrowed from the field of mechanics of rigid bodies. When a single force is applied at the C_RES, translation of the tooth in the direction of the line of action of the force occurs^1,2. The position of the C_RES depends not only on the tooth's anatomy and properties but also on its environment (e.g., periodontal ligament, surrounding bone, adjacent teeth). The tooth is a restrained body, making its C_RES similar to the center of mass of a free body. In the manipulation of appliances, most orthodontists consider the relationship of the force vector to the C_RES of a tooth or a group of teeth. Indeed, whether an object will display tipping or bodily movement when submitted to a single force is mainly determined by the location of the C_RES of the object and the distance between the force vector and the C_RES. If this can be accurately predicted, treatment results will be greatly improved. Thus, an accurate estimation of C_RES can greatly enhance the efficiency of orthodontic tooth movement.

For decades, the orthodontic field has been revisiting research regarding the location of the C_RES of a given tooth, segment, or arch^{1,2,3,4,5,6,7,8,9,10,11,12}. However, these studies have been limited in their approach in many ways. Most studies have determined the C_RES for only a few teeth, leaving out the majority. For example, the maxillary central incisor and the maxillary incisor segment have been evaluated quite extensively. On the other hand, there are only a few studies on the maxillary canine and first molar and none for the remaining teeth. Also, many of these studies have determined the location of the C_RES based on generic anatomical data for teeth, measurements from two-dimensional (2D) radiographs, and calculations on 2D drawings⁸. In addition, some of the current literature uses generic models or three-dimensional (3D) scans of dentiform models rather than human data^4,8. As orthodontics shifts into 3D technology for planning tooth movement, it is crucial to revisit this concept to develop a 3D, scientific understanding of tooth movement.

With technological advancements resulting in increased computational power and modeling capabilities, the ability to create and study more complex models has increased. The introduction of computed tomography scanning and cone-beam computed tomography (CBCT) scanning has thrust models and calculations from the 2D world into 3D. Simultaneous increases in computing power and software complexity have allowed researchers to use 3D radiographs to extract accurate anatomical models for use in advanced software to segment the teeth, bone, periodontal ligament (PDL), and various other structures^{7,8,9,10,13,14,15}. These segmented structures can be converted into a virtual mesh for use in engineering software to calculate the response of a system when a given force or displacement is applied to it.

This study proposes a specific, replicable methodology that can be utilized to examine hypothetical orthodontic force systems applied on models derived from CBCT images of live patients. In utilizing this methodology, investigators can then estimate the C_RES of various teeth and take into consideration the biological morphology of dental structures, such as tooth anatomy, number of roots and their orientation in 3D space, mass distribution, and structure of periodontal attachments. A general outline of this process is shown in Figure 1. This is to orient the reader to the logical process involved in generation of 3D tooth models for locating the C_RES.

Protocol

An institutional review board exemption was obtained for evaluating CBCT volumes archived in the Division of Oral and Maxillofacial Radiology (IRB No. 17-071S-2).

1. Volume selection and criteria

1. Acquire a CBCT image of the head and face¹⁶.
2. Examine the image for tooth alignment, missing teeth, voxel size, field of view, and overall quality of the image.
3. Make sure the voxel size is not larger than 350 µm (0.35 mm).

2. Segmentation of the teeth and bone

1. Load the raw DICOM files of the CBCT image into Mimics software for segmentation (Figure 2). Click Image > Crop Project. Crop the image to include only the maxilla and maxillary teeth.
   NOTE: The field of view should be large enough to capture the maxilla and maxillary teeth. Make sure the image includes the tooth crowns, the hard palate up to the nasal floor, maxillary sinuses, facial surfaces of the maxillary teeth, and the posterior extent of the hard palate and maxillary tuberosity.
2. Right click on the tab for Mask and create a New Mask for the image. Rename the mask as UL1, UL2, …, UL7 for the left side and UR1, UR2, …, UR7 for the right side, based on the tooth of interest.
3. Identify the tooth of interest on the masked CBCT image (see views). Use the Clear Mask tool to erase the mask. The software might be unable to distinguish between the teeth and bone because the gray values of the two are similar.
   NOTE: The thresholding tool in Mimics is unable to segment the teeth and bone separately. Therefore, a different method for segmentation is required.
4. Click on the Multiple Slice Edit tool (Ctrl + M). Select the view (Axial, Coronal, or Sagittal). Manually highlight (i.e., draw) some of the slices as deemed necessary.
   NOTE: Highlighting more slices adds more detail to the structure.
5. Click the Interpolate tool to fill up the volume for the skipped slices and apply.
6. Generate the 3D volume for the tooth by right-clicking on the mask and selecting the option to calculate the 3D volume.
7. Repeat steps 2.2-2.6 for each tooth of the maxillary arch.
8. Select all the 3D maxillary teeth, UL7-UR7. Right-click to select Smoothing. Set the smoothing factor to 0.4 and iterations to 4.
9. To segment the maxillary bones right-click on the tab for Mask. Create a new mask for the image.
10. From the drop-down menu for predefined threshold sets, select Custom. Adjust the threshold value to include the complete maxillary bone. Be sure to check the Fill Holes box before applying the threshold.
    NOTE: Small holes of ≤1 mm in the cortical bone are acceptable, because they can be removed easily in later stages.
11. Click on the Dynamic Region Growing Tool to fill the large holes visible in the mask. Select the maxillary bone mask as the target for the tool in addition to selecting the Multiple Layer box. Use 50 for the Min and 150 for Max values. Hold down the Control key while clicking on the areas of cortical bone that were not highlighted in the mask.
12. Right-click on the maxillary bone mask for the Smooth Mask function. Repeat this step 3x for best results.
13. Generate the 3D volume for the maxilla by right-clicking on the mask and selecting the option to calculate the 3D volume.
14. Select the 3D maxillary bone. Right-click to select smoothing. Set the smoothing factor to ~0.4 and iterations to 4.
15. Select the 3D maxillary bone and right-click to select Wrap. Set 0.2 mm for the smallest detail and 1 mm for the gap closing distance. Check the Protect Thin Walls option. Press Ok.
16. Rename the 3D maxillary bone "Maxilla".

3. Cleaning and meshing

1. Select the 3D objects and copy (Ctrl + C).
2. Open the 3matic software, and paste (Ctrl + V) the selected 3D objects. They will appear in the object tree and work area of 3matic as a 3D structure (Figure 3).
3. Click the Fix tab from the tool bar and use the Smooth option. Under the Operations box select the desired 3D object(s) or entities and Apply the default parameters.
4. Click the Finish tab from the tool bar and use the Local Smoothing option. Under the Operations Box select the desired 3D object(s) or entities. Use the cursor to manually smoothen out the desired regions.
5. Duplicate the teeth. On the object tree select all teeth, right-click, and select Duplicate.
6. Select All Duplicated Teeth, group, and name the folder "group 1". The original set will serve as the final teeth for analysis.
7. For the duplicated teeth in group 1, click the Curve Module and the Create Curve option. Manually draw a curve around the cementoenamel junction (CEJ) for all duplicated teeth.
8. Select the Curve, Contour, and Border entities under the Smooth Curve option.
9. Separate the crown and root surfaces into their own parts by selecting the Split Surfaces by Curves option and left-clicking on the 3D object to select.
10. Generate the PDL from the root structure of the tooth by splitting the tooth into root and crown at the CEJ.
    1. Duplicate the 3D objects from group 1 (generated in step 3.6) as group 2. For group 2, in the object tree box, click on the Object. From the surface list delete the crown surface. Perform this step for all objects in group 2.
    2. For group 2, click on Design Module > Hollow. Apply the desired parameters (Table 1).
    3. Click on the Fix Module > Fix Wizard. Click on the individual parts, update, and follow the given directions.
    4. Repeat step 3.10.3 for all parts. Rename all parts in the group 2 as "UL1_PDL" to "UL7_PDL" and "UR1_PDL" to "UR7_PDL".
11. In group 1, from the object tree box, click on Object. From the surface list delete the root surface.
12. Select Fill Hole Normal option and select the contour. Click on Bad Contour and Apply. The entire space will be filled.
13. Select the Design Module > Local Offset and select the entire crown surface. Check the following options: Direction (select external), Offset Distance (select 0.5), and Diminishing Distance (select 2.0). Apply.
14. Repeat step 3.13.
15. Repeat steps 3.11-3.14 for each tooth of the maxillary arch.
16. Remesh (Figure 3)
    1. Click the Remesh Module > Create Non-Manifold Assembly > Main Entity > Maxilla from the object tree. Select intersecting entity for all objects from 3.4 (original teeth) and select Apply.
    2. Click the Remesh Module. Split the non-manifold assembly.
    3. Repeat steps 3.16.1-3.16.2 using an intersecting entity as all objects from group 1 and Apply.
    4. As an optional step, only if required, select the Finish Module > Trim > Entity > Maxilla. Select the excess structure (i.e., noise) and Apply.
    5. Click the Fix Module > Fix Wizard > Maxilla > Update. Follow the directions given.
    6. Repeat step 3.16.1 using an intersecting entity as all objects from group 2 and Apply.
    7. Click the Remesh Module > Adaptive Remesh. Select all intersecting entities from 3.16.6 and Apply.
    8. Click the Remesh Module > Split Non-manifold Assembly.
    9. Click the Remesh Module > Create Non-manifold Assembly > Main Entity > Individual Object (PDL) from group 2 from the object tree. Select Intersecting Entity > Select Respective Object from step 3.4 (corresponding to that tooth type) and Apply.
    10. Click Remesh Module > Adaptive Remesh. Select the intersecting entity from 3.16.9 and Apply.
    11. Click Remesh Module > Split Non-manifold Assembly.
    12. Repeat steps 3.16.9-3.16.11 for each tooth.
17. Click the Remesh Module > Quality Preserving Reduce Triangles. In the object tree select all entities (i.e., teeth, PDLs, and Maxilla) and Apply.
18. Click Remesh Module > Create Volume Mesh > Select Entity. Choose Mesh Parameters.
19. Repeat step 3.18 for all entities (i.e., teeth, PDLs, and Maxilla).
20. Manually export the input(.inp) files from 3Matic to Abaqus (Figure 4).

4. Finite element analysis

NOTE: All custom Python scripts can be found in the supplemental attachments. They have been generated using the macro manager function in Abaqus.

1. Preprocessing setup
   1. Open Abaqus and select Standard Model. Click File > Set the Work Directory > Select Location for File Storage.
   2. Click File > Run Script and select Model_setup_Part1.py
   3. In the Model Directory specify the file path to load .inp files on Abaqus.
   4. Click on Models > Simulation > Parts > Maxilla > Surfaces.
   5. Name the surface in the dialog box "UL1 _socket".
   6. Under Select the Region of the Surface choose By Angle. Add "15" as the angle.
   7. Make sure all areas of the socket are selected. Press Done when completed.
   8. Repeat steps 4.1.4-4.1.7 for the individual sockets.
   9. Click on Models > Simulation > Parts. Then select UL1 > Surfaces. Name the surface "UL1".
   10. Under Select the Region of the Surface opt for "Individually". Select the tooth on the screen and press Done.
   11. Repeat steps 4.1.9-4.1.10 for all teeth.
   12. Click on Models > Simulation > Parts. Then select UL1_PDL > Surfaces. Name the surface "UL1_PDL_inner".
   13. Under Select the Region of the Surface choose By Angle. Add "15" as the angle.
       NOTE: If an error is found during the final simulation, reduce the angle and reselect the surface.
   14. Make sure the entire inner surface area of the PDL is selected. Press Done when completed.
   15. Select UL1_PDL > Surfaces. Name the surface "UL1_PDL_outer".
   16. Under Select the Region of the Surface choose By Angle. Add "15" as the angle.
       NOTE: If an error is found during the final simulation, reduce the angle and reselect the surface.
   17. Make sure the entire outer surface area of the PDL is selected. Press Done when completed.
   18. Repeat steps 4.1.13-4.1.19 for all PDLs.
   19. Click on File > Run Script and select Model_setup_Part2.py
   20. Click on Models > Simulation > BCs. Name BC_all, then select Step as Initial. Under category, select "Mechanical", and under "Types of Selected Step" select "Displacement/Rotation". Press Continue.
   21. Under Select Regions for the Boundary Condition select By Angle. Add "15" as the angle. Check Create Set. Select individual sockets for the 14 teeth. Press Done.
       NOTE: This helped simulate instantaneous tooth movement.
   22. Click on Models > Simulation > Assembly > Sets > Create Set. Name the set "U1_y_force".
   23. In Select the Nodes for the Set choose Individually.
       NOTE: A one Newton concentrated force was applied on a randomly selected tooth node in either the positive Y direction (simulating a distalization force) or the positive Z direction (simulating an intrusive force).
   24. Select a node at the center of the crown on the buccal surface of the upper central incisor (U1) and press Done.
   25. Click Sets > Create Set. Name the set "U1_z_force".
   26. Repeat steps 4.1.23-4.1.24.
   27. Repeat steps 4.1.22-4.1.26 for all teeth.
       NOTE: Before a set is generated for a particular tooth as in 4.1.25, go to Instance > Resume for that tooth.
2. Model set up
   1. Click on Models > Simulation > Assembly > Instances. Select All Instances and click Resume.
   2. Click on Tools > Query > Point/Node. Select a node at the center of a randomly selected central incisor and press Done.
   3. Under the command center at the bottom of the page, copy the X, Y, and Z coordinates of the node selected in step 4.2.2.
   4. Under the vertical tool bar select Translate Instance and select the entire assembly (i.e., all instances) on the screen. Press Done.
   5. In the Select a Start Point for the Translation Vector box, paste the copied coordinates in step 4.2.3 or enter the X, Y, and Z values. Click Enter.
   6. Under Select an End Point for the Translation Vector or enter X,Y,Z: enter the coordinates "0.0", "0.0", and "0.0". Click Enter.
   7. For Position of Instance, press Ok.
   8. Click on Tools > Query > Point/Node and select a node directly above the midline of the center incisors. Enter Done.
   9. Under the command center at the bottom of the page, copy the X, Y, and Z coordinates of the node selected in step 4.2.8.
   10. Under the vertical tool bar select Translate Instance and select the entire assembly (i.e., all instances) on the screen. Enter Done.
   11. Paste the copied coordinates into the Select a Start Point for the Translation Vector - or Enter X,Y,Z box. Click Enter.
   12. Under Select an End Point for the Translation Vector - or enter X,Y,Z: insert the coordinates as copied in step 4.2.9. Change the X coordinate to 0.0. Click Enter.
   13. For Position of Instance, press Ok.
   14. Click on File > Run Script and select Model_setup_Part3.py. Insert or change material properties.
   15. Click on Models > Simulation > Materials and click Bone/PDL/Tooth. Insert tissue specific properties.
   16. Click on File > Run Script and select Functions.py.
3. Processing the model
   1. Click on File > Run Script and select Job_submission.py.
      NOTE: The job module is where the user sets up one or more actions on the model, and job manager is where model analysis is started, progress is shown, and completion is noted.
   2. In the dialog box titled Suppress All, enter the sides (L or R) of the teeth based on constraints (Under Models > Simulation > Constraints). Press Ok.
   3. In the dialog box titled Job Submission enter "Y" to run the analysis for the specified tooth/teeth. Press Ok.
   4. In the dialog box titled Directions for Analysis enter "Y" to specify force application. Press Ok.
4. Post processing for C _RES estimation
   1. Choose File > Run Script > Bulk_process.py.
   2. In the dialog box titled Analyze Multiple Jobs enter "Y" for the specified tooth/teeth. Press Ok.
   3. In the dialog box titled Directions for Analysis enter "Y" for specifying force application. Press Ok.
   4. In the dialog box titled Get Input enter Specific Tooth Number as outlined named Instances (e.g., UL1 or UL5, etc.). Press Ok.
   5. Check coordinates for the Force About Point and Estimated Location in the command box. If they are not similar, then repeat steps 4.3.1-4.4.4.
      NOTE: After the jobs for each step were run, a user-defined algorithm created in Python was run within the Abaqus interface to analyze the reaction force system and subsequent moments created as a result of load application. The algorithm automatically suggests a new node location to apply the load such that a moment of near-zero magnitude is created within the force system. This proceeds in an iterative process, until the node location that creates a moment closest to zero when a force is applied through it is found or estimated. The algorithm is described in detail in the Discussion section.

Results

In order to verify segmentation and manual outlining as described in the Procedures section (step 2), a maxillary first molar was extracted from a dry skull, and a CBCT image was taken. The image processing and editing software Mimics was used for manually outlining the tooth as described in step 2. Subsequently, meshing was performed, the segmented models were cleaned with 3matic software, and they were imported to Abaqus for analysis. We did not find any significant difference in the li...

Discussion

This study shows a set of tools to establish a consistent workflow for finite element analysis (FEA) of models of maxillary teeth derived from CBCT images of patients to determine their C_RES. For the clinician, a clear and straightforward map of the C_RES of the maxillary teeth would be an invaluable clinical tool to plan tooth movements and predict side effects. The finite element method (FEM) was introduced in dental biomechanical research in 1973¹⁷, and since then has been ...

Materials

List of materials used in this article

Name	Company	Catalog Number	Comments
3-matic software	Materialise, Leuven, Belgium.		Cleaning and meshing
Abaqus/CAE software, version 2017	Dassault Systèmes Simulia Corp., Johnston, RI, USA.		Finite Element Analysis
Mimics software, version 17.0	Materialise, Leuven, Belgium.		Segmentation of teeth and bone