这项研究得到了美国正畸医师协会基金会 （AAOF） 正畸教师发展奖学金奖（针对 CL）、美国正畸医师协会 （AAO） 全职教师奖学金（针对 CL）、宾夕法尼亚大学牙科医学院 Joseph 和 Josephine Rabinowitz 卓越研究奖（针对 CL）、正畸学系的 J. Henry O'Hern Jr. 试点资助， 宾夕法尼亚大学牙科医学院（C.L.）和国际正畸基金会青年研究基金（C.L.）。

本研究利用了一名患有 SARPE 的患者的预先存在的、去识别化的治疗前 CBCT 图像作为治疗计划的一部分。该研究是根据《赫尔辛基宣言》进行的，并得到了机构审查委员会（协议#853608）的批准。
1. 样本采集和牙齿分割
<ol><li>在自然头部位置获取头部的人类 CBCT 图像，包括患者的上颌骨复合体，包括上颌基底骨、上颌牙槽骨和上颌牙列。</li>
	<li>将 CBCT Digital Imaging and Communications in Medicine （DICOM） 文件导入 Mimics 软件。<ol><li>创建 新项目 （Ctrl + N），选择所有 DICOM 图像，然后单击 “下一步 ”和 “转换”。</li>
		<li>定义模型的方向（A：前方，P：后方，T：顶部，B：下部，L：左，R：右），然后单击 确定。</li>
	</ol></li>
	<li>将锉刀分割为上颌复合体、上颌第一前磨牙和上颌第一磨牙。<ol><li>单击阈值，选择适当的 阈值来分割骨骼，然后单击 应用。</li>
		<li>创建新面罩并单击“ 编辑面罩”，使用 “绘制 和 擦除 ”来分割患者的上颌骨复合体、上颌第一前磨牙和上颌第一磨牙。</li>
	</ol></li>
	<li>将目标导出为立体光刻 （STL） 文件。<ol><li>右键单击蒙版，然后选择 “计算 3D ”以生成 3D 对象。</li>
		<li>右键单击 3D 对象，选择 STL+，选择所需的对象，然后按 “添加 ”和 “完成 ”以创建 STL 文件。</li>
	</ol></li>
</ol>2. 表面平滑和形成松质骨和牙周韧带间隙
<ol><li>将 STL 文件导入 Geomagic 软件。<ol><li>单击 “文件”>“打开”，选择 STL 文件，然后按 “打开”。</li>
		<li>为单位中的数据弹出窗口选择“毫米”，然后单击“确定”。</li>
	</ol></li>
	<li>平滑上颌复合体、上颌第一前磨牙和上颌第一磨牙的表面。<ol><li>单击 “多边形”>“移除尖峰”，单击“ 低”附近的平滑度级别并将其拖动，单击 “应用”，然后单击“ 确定”。</li>
		<li>单击 “多边形”>“松弛多边形”，单击并拖动“ 最小”附近的平滑度级别，单击 “应用”，然后单击“ 确定”。</li>
		<li>单击“多边形”>“修复交叉点”，在“模式”窗口中选择“放松/清洁”，单击“应用”，然后单击“确定”。</li>
	</ol></li>
	<li>将模型的曲面修改为连续的闭合区域。<ol><li>单击并拖动锐曲面，然后按 Delete 键以创建孔。</li>
		<li>单击“填充孔”>“多边形”，在“填充方法”窗口中使用“填充”、“填充部分”、“创建桥梁”来填充孔，然后单击“应用”，然后单击“确定”。</li>
	</ol></li>
	<li>将 2D 曲面转换为 3D 实体模型，并将其导出为计算机辅助设计 （CAD） 文件。<ol><li>单击“ 编辑”>“相位”>“形状相位”，选择 “编辑轮廓 ”以草绘曲面的轮廓，然后单击“ 确定”。</li>
		<li>单击“绘制面片布局”（Draw Patch Layout） 并绘制四边形网格以覆盖所有曲面，然后单击“确定”（OK）。</li>
		<li>单击 “构造网格”（Construct Grids），定义适当的“分辨率”（ Resolution），然后单击 “确定 ”（OK） 以生成更精细的网格。</li>
		<li>单击 “拟合曲面”（Fit Surfaces），单击“应用”（Apply），然后单击“ 确定”（ OK ） 以构建 3D 实体模型。</li>
		<li>单击 “文件”（File） >“另存为”（Save as ） 以输出 3D 模型并将其保存在 IGES 文件（名为 Maxilla）中。</li>
	</ol></li>
	<li>通过将上颌复合体的体积从颊牙槽表面减少 1 毫米来创建松质骨。通过将牙根的轮廓扩大 0.2 毫米来创造牙周韧带空间。<ol><li>单击“面相位”（Polygon Phase），在“等值线”（Contour Lines） 窗口中选择“删除”（Delete），在“Patch 布局”窗口中选择“保留”（Preserve），然后按“确定”（OK） 将 3D 实体模型转换为 2D 曲面。</li>
		<li>单击 多边形>偏移，在松质骨和牙周韧带的距离面板中输入 -1 mm 和 0.2 mm，然后单击 应用 和 确定。</li>
		<li>单击 Edit > Phase > Shape Phase，选择 Restore Patch Layout，然后按 OK。</li>
		<li>单击 “构造网格”（Construct Grids），定义适当的“分辨率”（ Resolution），然后单击 “确定 ”（OK） 以生成更精细的网格。</li>
		<li>单击 “拟合曲面”（Fit Surfaces），单击“应用”（Apply），然后单击“ 确定”（ OK ） 以构建 3D 实体模型。</li>
		<li>单击“ 文件”（File） >“另存为”（Save as ） 以输出 3D 模型并将其保存在 IGES 文件（名为 CB 和 PL）中。</li>
	</ol></li>
</ol>3. 构建解剖对称上颌骨模型
<ol><li>将 CAD 文件输入到 SolidWorks 中。<ol><li>单击 “文件”>“打开”，选择上颌骨文件，然后按 “打开 ”导入 CAD 文件。</li>
		<li>单击 “文件”>“保存 ”将文件保存为 “部件 ”格式。</li>
	</ol></li>
	<li>在腭平面 （PP） 下方构建松质骨。<ol><li>单击“ 插入>零件”，选择 CB 文件，然后按 “打开 ”导入 CAD 文件。</li>
		<li>单击“ 插入>参照几何>平面”（Plane ），在腭面上选取三个特征点，然后单击 “确定 ”（OK） 以创建切割平面。</li>
		<li>单击 “插入>特征”>“分割”，在 “修剪工具”中选择腭平面，然后单击“切割零件”以创建 切割 预览。</li>
		<li>勾选 “生成的实体”中的复选框，然后单击“ 确定 ”以分离松质骨。</li>
		<li>单击腭平面上方的松质骨，右键单击并按“正文”部分中的“删除”。</li>
	</ol></li>
	<li>构建上颌第一前磨牙和上颌第一磨牙的牙周韧带。<ol><li>单击 “插入零件>”（Insert Part），选择 PL 文件，然后按“ 打开 ”（Open） 导入 CAD 文件。</li>
		<li>单击“ 插入”>“特征”>“相交”，然后在 “选择 ”窗口中选择“上颌和PL”。</li>
		<li>在“选择”窗口中选择“同时创建”，在“区域列表”中选择牙周韧带部分，然后单击“确定”以生成韧带。</li>
	</ol></li>
	<li>执行从前鼻棘 （ANS） 到后鼻棘 （PNS） 的腭中部切割平面，并保留上颌复合体的右半部分。<ol><li>单击“ 插入>参照几何”>平面“（Insert Reference Geometry），在腭中平面上选取三个特征点，然后单击”确定“（ OK ） 创建切割平面。</li>
		<li>单击“ 插入”>“特征”>“分割”，在 “修剪工具”中选择腭平面，然后单击 “切割零件 ”以创建切割预览。</li>
		<li>勾选“ 生成的实体”中的复选框，然后单击 “确定 ”以分离上颌复合体。</li>
		<li>单击上颌复合体的左半部分，单击鼠标右键，然后按“正文”部分中的“删除”。 </li>
	</ol></li>
	<li>镜像上颌复合体的右半部分并创建一个相同的左半部分。<ol><li>单击“ > Mirror > Mirror”中插入图案/镜像，然后在 “镜像面/面”中选择中腭平面。</li>
		<li>在 要镜像的身体中选择所有右半上颌复合体，然后单击 确定 以生成上颌复合体的左半部分。</li>
	</ol></li>
</ol>4. 在上颌第一前磨牙和第一磨牙上创建一个 Haas 扩张器和束带
<ol><li>构建前磨牙带和磨牙带。<ol><li>单击 “插入零件”（Insert > Part），选择 PL 文件，然后按“ 打开 ”（Open） 导入 CAD 文件。</li>
		<li>单击“ 插入>特征”>“分割”，选择 PL 文件中的齿，并将 “均匀缩放 ”设置为 1.05。单击 “确定 ”（OK） 生成厚度为 0.5 mm 的条带。</li>
		<li>单击“ 插入>参考几何>平面”，在遮挡平面上选择三个特征点，然后单击 “确定 ”以创建参考平面。</li>
		<li>单击“ 插入>参照几何>平面”（Reference Geometry Plane），选择遮挡平面，并将偏移距离设置为 1.5 mm。单击 “确定 ”（OK） 创建第一个切割平面。</li>
		<li>单击 “插入>参照几何>平面”（Plane ），选择遮挡平面，并将偏移距离设置为 4.0 mm。单击 “确定 ”（OK） 创建第二个切割平面。</li>
		<li>单击“ 插入”>“特征”>“分割”，然后在 “修剪工具”（Trim Tools ） 中选取第一个和第二个平面，并在 “目标主体”（Target Bodies） 中选取齿。单击 “切割主体”（Cut Bodies ） 以创建切割预览。</li>
		<li>勾选“ 生成的实体”中的复选框，然后单击 “确定 ”以分离齿。</li>
		<li>单击第一个平面上方和第二个平面下方的波段，单击鼠标右键，然后按“正文”部分中的“删除”。 </li>
	</ol></li>
	<li>构建亚克力板。<ol><li>单击“ 插入>参照几何>平面”（Insert Reference Geometry），在硬腭平面上选取三个特征点，然后单击“确定”（ OK ） 创建草图平面。</li>
		<li>单击 “插入”>“草图”，绘制参考 Haas 扩展器的亚克力板，然后单击 “退出草图”。</li>
		<li>单击“ 插入”>凸台/底座>“拉伸”，选择亚克力板的草图，在 “深度”中设置 5 mm，然后单击 “确定”。</li>
		<li>单击 “插入>特征”>“弯曲”，然后弯曲亚克力板以适应上颚的解剖结构。</li>
		<li>单击 “插入>特征”（Insert Features > Fillet/Round“（圆角/圆形），然后在半径为 1 mm 的范围内对亚克力板的锋利边缘进行圆角。</li>
	</ol></li>
	<li>构造扩张臂。<ol><li>单击“ 插入>参照几何”>平面“（Plane ），在波段上选取三个特征点，然后单击 ”确定 “（OK） 以创建草图平面（命名为 P1）。</li>
		<li>单击“ 插入草绘”>，绘制一个直径为 2 mm 的圆，然后单击“ 退出草绘 ”（名为 C1）。</li>
		<li>单击“ 插入>参照几何体>平面”，在亚克力板上选择三个特征点，然后单击 “确定 ”以创建草图平面（命名为 P2）。</li>
		<li>单击 “插入”>“草绘”，绘制一个直径为 2 mm 的圆，然后单击“ 退出草绘 ”（名为 C2）。</li>
		<li>单击“ 插入>参照几何>平面”（Insert Reference Geometry），选取 P2 平面，并将偏移距离设置为 6 mm。单击 “确定 ”（OK） 进入草绘平面。</li>
		<li>单击“ 插入草绘”（Sketch>），绘制一个直径为 2 mm 的圆，然后单击“ 退出草绘”（Exit Sketch ）（名为 C3）。</li>
		<li>单击“ 插入”>“凸台/底座”>放样“，然后在 ”截面梁“（Profiles ） 窗口中选取 C1、C2 和 C3 草图。</li>
		<li>在“特征范围”窗口中选择波段和亚克力板，勾选“选项”窗口中的“合并结果”，然后单击“确定”。</li>
	</ol></li>
</ol>5. 设计截骨术
<ol><li>创建一个 1 毫米厚的平面，相当于外科医生通常使用的车针直径，从梨状孔 （Alar） 的角到颧下嵴 （IZC） 从水平面不同角度。<ol><li>单击“ 插入>参考几何>平面”，在截骨平面上选择三个特征点（与水平面成 0°、10°、20° 或 30°），然后单击“ 确定 ”以创建平面（命名为 O1）。</li>
		<li>单击“ 插入>参照几何>平面”（Insert Reference Geometry），选择截骨平面，并将偏移距离设置为 1.0 mm。单击 “确定 ”（OK） 创建下部切割平面（命名为 O2）。</li>
		<li>单击“ 插入”>“特征”>“分割”，在 “修剪工具”中选择“O1”和“O2”平面，然后单击 “切割零件 ”以创建切割预览。</li>
		<li>勾选“ 生成的实体”中的复选框，然后单击 “确定 ”以分离上颌复合体。</li>
		<li>单击 O1 和 O2 平面之间的主体，单击鼠标右键，然后在主体部分中按 Delete 键。</li>
	</ol></li>
	<li>在 Parasolid 模型零件文件 （X_T） 中导出具有不同颊骨截骨角度的模型以进行分析。<ol><li>单击“文件”>“另存为”，然后在“文件类型”列表中选择“Parasolid （x_t）”。</li>
		<li>单击 “保存 ”以导出有限元分析软件的模型。</li>
	</ol></li>
</ol>6. 有限元分析
<ol><li>将上颌骨复杂模型的材料参数导入并设置到Ansys软件中。<ol><li>单击并拖动“工具箱中的静态结构”以创建分析工作空间。</li>
		<li>双击工程数据，然后在属性中设置所有材料的杨氏模量和泊松比。不同结构12、15、16的材料性能列于表1中。</li>
		<li>双击 “几何”，单击 “文件”>“导入外部几何文件”，然后单击 “生成 ”以导入上颌复杂模型。</li>
		<li>单击“ 创建>布尔值”，然后用松质骨和牙齿生成皮质骨和牙周韧带。</li>
	</ol></li>
	<li>设置有限元分析模型。<ol><li>双击 “模型”（Model），然后单击 “几何”（Geometry ） 以选择每个零件的材料属性。</li>
		<li>右键单击“网格”（ Mesh ），然后单击 “生成网格”（Generate Mesh ） 以在模型上构建单元。</li>
		<li>单击 “连接”（Connections），在“ 接触主体 ”（Contact Bodies） 中指定软/小零件，在 “目标实体”（Target Bodies） 中指定刚性/大零件。</li>
		<li>在“定义”中指定接触类型和摩擦系数。表2列出了不同部件17的连接特性。</li>
		<li>右键单击“ 连接”，单击“ 插入>弹簧 ”以连接截骨平面的上部和下部。将弹簧设置为 1 mm 长，弹簧常数 k = 60 N/mm，并在每个网格节点处放置一个弹簧。</li>
	</ol></li>
	<li>在各种截骨组合上沿亚克力板上的x轴（垂直于中线）设置临床上可接受的力。<ol><li>右键单击 “静态结构”（Static Structural），单击 “插入>固定支撑”（Fixed Support ），并将腭面上的结构设置为不可移动。</li>
		<li>右键单击 “静态结构”（Static Structural），单击 “插入> 力”（Insert Force），然后设置一个 150 N 的力以施加在远离内线的方向的亚克力板上。</li>
		<li>右键单击 “求解”（Solution），然后单击 “插入>变形”（Deformation > Total ） 以监视展开的变形。</li>
	</ol></li>
	<li>进行收敛测试，直到实现两端的扩展。<ol><li>单击工具栏上的 “求解 ”（Solve），然后等待“力收敛”（Force Convergence） 级别达到 “力标准”（Force Criterion）。</li>
		<li>单击 “总变形”（Total Deformation ） 以显示展开结果。</li>
	</ol></li>
	<li>测量解剖标志在所有三个维度上的位移，作为扩张的结果。建议使用以下地标来评估扩展模式： 上颌中切牙 （U1） 的近切线角。 上颌第一前磨牙（U4）的颊尖。 上颌第一磨牙（U6）的近中颊尖。 梨状孔（Alar）的外侧下角。 颧下嵴 （IZC）。 扩张器的中点。</li>
</ol>

使用有限元模型分析 SARPE 的膨胀模式

<ol>
	<li>Mommaerts, M. Y. <a target="_blank" href="http://www.ncbi.nlm.nih.gov/entrez/query.fcgi?db=PubMed&cmd=Search&doptcmdl=Citation&defaultField=Title+Word&term=Transpalatal+distraction+as+a+method+of+maxillary+expansion.">Transpalatal distraction as a method of maxillary expansion.</a> British Journal of Oral and Maxillofacial Surgery. 37 (4), 268-272 (1999).</li><li>Betts, N. J., Vanarsdall, R. L., Barber, H. D., Higgins-Barber, K., Fonseca, R. J. <a target="_blank" href="http://www.ncbi.nlm.nih.gov/entrez/query.fcgi?db=PubMed&cmd=Search&doptcmdl=Citation&defaultField=Title+Word&term=Diagnosis+and+treatment+of+transverse+maxillary+deficiency.">Diagnosis and treatment of transverse maxillary deficiency.</a> The International Journal of Adult Orthodontics and Orthognathic Surgery. 10 (2), 75-96 (1995).</li><li>Lin, J. H., et al. <a target="_blank" href="http://www.ncbi.nlm.nih.gov/entrez/query.fcgi?db=PubMed&cmd=Search&doptcmdl=Citation&defaultField=Title+Word&term=Asymmetric+maxillary+expansion+introduced+by+surgically+assisted+rapid+palatal+expansion:+A+systematic+review.">Asymmetric maxillary expansion introduced by surgically assisted rapid palatal expansion: A systematic review.</a> Journal of Oral and Maxillofacial Surgery. 80 (12), 1902-1911 (2022).</li><li>Chamberland, S., Proffit, W. R. <a target="_blank" href="http://www.ncbi.nlm.nih.gov/entrez/query.fcgi?db=PubMed&cmd=Search&doptcmdl=Citation&defaultField=Title+Word&term=Short-term+and+long-term+stability+of+surgically+assisted+rapid+palatal+expansion+revisited.">Short-term and long-term stability of surgically assisted rapid palatal expansion revisited.</a> American Journal of Orthodontics and Dentofacial Orthopedics. 139 (6), 815-822 (2011).</li><li>Verlinden, C. R., Gooris, P. G., Becking, A. G. <a target="_blank" href="http://www.ncbi.nlm.nih.gov/entrez/query.fcgi?db=PubMed&cmd=Search&doptcmdl=Citation&defaultField=Title+Word&term=Complications+in+transpalatal+distraction+osteogenesis:+a+retrospective+clinical+study.">Complications in transpalatal distraction osteogenesis: a retrospective clinical study.</a> Journal of Oral and Maxillofacial Surgery. 69 (3), 899-905 (2011).</li><li>de Assis, D. S., et al. <a target="_blank" href="http://www.ncbi.nlm.nih.gov/entrez/query.fcgi?db=PubMed&cmd=Search&doptcmdl=Citation&defaultField=Title+Word&term=Finite+element+analysis+of+stress+distribution+in+anchor+teeth+in+surgically+assisted+rapid+palatal+expansion.">Finite element analysis of stress distribution in anchor teeth in surgically assisted rapid palatal expansion.</a> International Journal of Oral and Maxillofacial Surgery. 42 (9), 1093-1099 (2013).</li><li>Han, U. A., Kim, Y., Park, J. U. <a target="_blank" href="http://www.ncbi.nlm.nih.gov/entrez/query.fcgi?db=PubMed&cmd=Search&doptcmdl=Citation&defaultField=Title+Word&term=Three-dimensional+finite+element+analysis+of+stress+distribution+and+displacement+of+the+maxilla+following+surgically+assisted+rapid+maxillary+expansion.">Three-dimensional finite element analysis of stress distribution and displacement of the maxilla following surgically assisted rapid maxillary expansion.</a> Journal of Cranio-Maxillofacial Surgery. 37 (3), 145-154 (2009).</li><li>Lee, S. C., et al. <a target="_blank" href="http://www.ncbi.nlm.nih.gov/entrez/query.fcgi?db=PubMed&cmd=Search&doptcmdl=Citation&defaultField=Title+Word&term=Effect+of+bone-borne+rapid+maxillary+expanders+with+and+without+surgical+assistance+on+the+craniofacial+structures+using+finite+element+analysis.">Effect of bone-borne rapid maxillary expanders with and without surgical assistance on the craniofacial structures using finite element analysis.</a> American Journal of Orthodontics and Dentofacial Orthopedics. 145 (5), 638-648 (2014).</li><li>M&#246;hlhenrich, S. C., et al. <a target="_blank" href="http://www.ncbi.nlm.nih.gov/entrez/query.fcgi?db=PubMed&cmd=Search&doptcmdl=Citation&defaultField=Title+Word&term=Simulation+of+three+surgical+techniques+combined+with+two+different+bone-borne+forces+for+surgically+assisted+rapid+palatal+expansion+of+the+maxillofacial+complex:+a+finite+element+analysis.">Simulation of three surgical techniques combined with two different bone-borne forces for surgically assisted rapid palatal expansion of the maxillofacial complex: a finite element analysis.</a> International Journal of Oral and Maxillofacial Surgery. 46 (10), 1306-1314 (2017).</li><li>Nowak, R., Olejnik, A., Gerber, H., Fr&#261;tczak, R., Zawi&#347;lak, E. <a target="_blank" href="http://www.ncbi.nlm.nih.gov/entrez/query.fcgi?db=PubMed&cmd=Search&doptcmdl=Citation&defaultField=Title+Word&term=Comparison+of+tooth-+and+bone-borne+appliances+on+the+stress+distributions+and+displacement+patterns+in+the+facial+skeleton+in+surgically+assisted+rapid+maxillary+expansion-A+finite+element+analysis+(FEA)+study.">Comparison of tooth- and bone-borne appliances on the stress distributions and displacement patterns in the facial skeleton in surgically assisted rapid maxillary expansion-A finite element analysis (FEA) study.</a> Materials (Basel). 14 (5), 1152 (2021).</li><li>Shi, Y., Zhu, C. N., Xie, Z. <a target="_blank" href="http://www.ncbi.nlm.nih.gov/entrez/query.fcgi?db=PubMed&cmd=Search&doptcmdl=Citation&defaultField=Title+Word&term=Displacement+and+stress+distribution+of+the+maxilla+under+different+surgical+conditions+in+three+typical+models+with+bone-borne+distraction:+a+three-dimensional+finite+element+analysis.">Displacement and stress distribution of the maxilla under different surgical conditions in three typical models with bone-borne distraction: a three-dimensional finite element analysis.</a> Journal of Orofacial Orthopedics/Fortschritte der Kieferorthopadie. 81 (6), 385-395 (2020).</li><li>Tomazi, F. H. S., et al. <a target="_blank" href="http://www.ncbi.nlm.nih.gov/entrez/query.fcgi?db=PubMed&cmd=Search&doptcmdl=Citation&defaultField=Title+Word&term=The+Hyrax+appliance+with+tooth+anchorage+variations+in+surgically+assisted+rapid+maxillary+expansion:+a+finite+element+analysis.">The Hyrax appliance with tooth anchorage variations in surgically assisted rapid maxillary expansion: a finite element analysis.</a> Oral and Maxillofacial Surgery. , (2022).</li><li>Trivedi, S. <a target="_blank" href="http://www.ncbi.nlm.nih.gov/entrez/query.fcgi?db=PubMed&cmd=Search&doptcmdl=Citation&defaultField=Title+Word&term=Finite+element+analysis:+A+boon+to+dentistry.">Finite element analysis: A boon to dentistry.</a> Journal of Oral Biology and Craniofacial Research. 4 (3), 200-203 (2014).</li><li>Sankar, S. G., et al. <a target="_blank" href="http://www.ncbi.nlm.nih.gov/entrez/query.fcgi?db=PubMed&cmd=Search&doptcmdl=Citation&defaultField=Title+Word&term=A+comparison+of+different+osteotomy+techniques+with+and+without+pterygomaxillary+disjunction+in+surgically+assisted+maxillary+expansion+utilizing+modified+hybrid+rapid+maxillary+expansion+device+with+posterior+implants:+A+finite+element+study.">A comparison of different osteotomy techniques with and without pterygomaxillary disjunction in surgically assisted maxillary expansion utilizing modified hybrid rapid maxillary expansion device with posterior implants: A finite element study.</a> National Journal of Maxillofacial Surgery. 12 (2), 171-180 (2021).</li><li>Han, U. A., Kim, Y., Park, J. U. <a target="_blank" href="http://www.ncbi.nlm.nih.gov/entrez/query.fcgi?db=PubMed&cmd=Search&doptcmdl=Citation&defaultField=Title+Word&term=Three-dimensional+finite+element+analysis+of+stress+distribution+and+displacement+of+the+maxilla+following+surgically+assisted+rapid+maxillary+expansion.">Three-dimensional finite element analysis of stress distribution and displacement of the maxilla following surgically assisted rapid maxillary expansion.</a> Journal of Craniomaxillofacial Surgery. 37 (3), 145-154 (2009).</li><li>Esen, A., Soganci, E., Dolanmaz, E., Dolanmaz, D. <a target="_blank" href="http://www.ncbi.nlm.nih.gov/entrez/query.fcgi?db=PubMed&cmd=Search&doptcmdl=Citation&defaultField=Title+Word&term=Evaluation+of+stress+by+finite+element+analysis+of+the+midface+and+skull+base+at+the+time+of+midpalatal+osteotomy+in+models+with+or+without+pterygomaxillary+dysjunction.">Evaluation of stress by finite element analysis of the midface and skull base at the time of midpalatal osteotomy in models with or without pterygomaxillary dysjunction.</a> British Journal of Oral &amp; Maxillofacial Surgery. 56 (3), 177-181 (2018).</li><li>Huzni, S., Oktianda, F., Fonna, S., Rahiem, F., Angriani, L. <a target="_blank" href="http://www.ncbi.nlm.nih.gov/entrez/query.fcgi?db=PubMed&cmd=Search&doptcmdl=Citation&defaultField=Title+Word&term=The+use+of+frictional+and+bonded+contact+models+in+finite+element+analysis+for+internal+fixation+of+tibia+fracture.">The use of frictional and bonded contact models in finite element analysis for internal fixation of tibia fracture.</a> Frattura ed Integrit&#224; Strutturale. 61, 130-139 (2022).</li><li>Holmes, D. <a target="_blank" href="http://www.ncbi.nlm.nih.gov/entrez/query.fcgi?db=PubMed&cmd=Search&doptcmdl=Citation&defaultField=Title+Word&term=Closing+the+gap.">Closing the gap.</a> Nature. 550 (7677), S194-S195 (2017).</li><li>Lombardo, L., et al. <a target="_blank" href="http://www.ncbi.nlm.nih.gov/entrez/query.fcgi?db=PubMed&cmd=Search&doptcmdl=Citation&defaultField=Title+Word&term=Evaluation+of+the+stiffness+characteristics+of+rapid+palatal+expander+screws.">Evaluation of the stiffness characteristics of rapid palatal expander screws.</a> Progress in Orthodontics. 17 (1), 36 (2016).</li><li>Zandi, M., Miresmaeili, A., Heidari, A., Lamei, A. <a target="_blank" href="http://www.ncbi.nlm.nih.gov/entrez/query.fcgi?db=PubMed&cmd=Search&doptcmdl=Citation&defaultField=Title+Word&term=The+necessity+of+pterygomaxillary+disjunction+in+surgically+assisted+rapid+maxillary+expansion:+A+short-term,+double-blind,+historical+controlled+clinical+trial.">The necessity of pterygomaxillary disjunction in surgically assisted rapid maxillary expansion: A short-term, double-blind, historical controlled clinical trial.</a> Journal of Cranio-Maxillofacial Surgery. 44 (9), 1181-1186 (2016).</li><li>M&#246;hlhenrich, S. C., et al. <a target="_blank" href="http://www.ncbi.nlm.nih.gov/entrez/query.fcgi?db=PubMed&cmd=Search&doptcmdl=Citation&defaultField=Title+Word&term=Three-dimensional+effects+of+pterygomaxillary+disconnection+during+surgically+assisted+rapid+palatal+expansion:+a+cadaveric+study.">Three-dimensional effects of pterygomaxillary disconnection during surgically assisted rapid palatal expansion: a cadaveric study.</a> Oral Surgery, Oral Medicine, Oral Pathology, and Oral Radiology. 121 (6), 602-608 (2016).</li></ol>

作者声明没有利益冲突。

SARPE 中颊骨切开术的方向可以是上颌骨支撑区域向下踩踏之前从鼻孔水平切开，也可以是从梨状边缘向上颌第一磨牙相对应的支撑的斜坡切口，如 Betts2 所述。无论哪种方式，截骨术都延伸到上颌骨的颧突下方。然而，目前大多数关于SARPE的有限元分析研究都使用水平切口，向后延伸，与梨状边缘6,7,12,14相同。</sup...

手术辅助快速腭扩张 （SARPE） 是一种常用的技术，用于骨骼成熟患者的上颌骨结构和牙弓横向扩张1.该手术包括 LeFort I 截骨术、腭中皮质切开术，以及翼上颌裂2 的松解术。然而，已有报道称，SARPE 不希望的扩张模式，例如左半上颌骨和右半上颌骨3 之间的不均匀扩张和牙槽突颊侧倾/旋转4，这可能导致 SARPE 失败，有时甚至需要额外的手术进行矫正5。先前的研究表明，上颌周截骨术的变化可能在 SARPE 扩张后模式中起重要作用2,3，因为 Le Fort I 截骨部位的骨块之间的碰撞会导致半上颌骨横向扩张的不均匀阻力和半上颌骨的旋转，切口下方的牙槽边缘向内移动，而牙槽突扩张 3，4.因此，有必要研究不同截骨方向，尤其是颊骨截骨术对 SARPE 后扩张模式的影响。
已经建立了几个有限元分析（FEA）模型来评估SARPE过程中的力分布。然而，这些模型中的膨胀量限制在最多 1 mm，远低于所需的临床量 6,7,8,9,10,11,12。FEA 模型的扩展不足可能导致对 SARPE 后结果的错误预测。更具体地说，正如 Chamberland 和 Proffit4 所报道的那样，如果扩张器没有充分转动，可能无法证明截骨部位的骨骼之间的碰撞，这可能不能反映真实的临床现实。由于先前模型中内置的扩展量有限，因此这些模型的结果评估集中在应力分析上。然而，牙科中有限元分析的应力分析通常是在静态载荷下进行的，材料的力学性能设置为各向同性和线性弹性，这进一步限制了有限元分析研究的临床相关性13。
此外，这些研究中的大多数没有考虑截骨部位6、7、8、10、11、12 处的手术器械厚度，通常将切口处的摩擦设置为零作为边界条件的一部分。然而，这种设置过度简化了硬组织和软组织之间的接触。它可能会显着影响力的分布和由此产生的半上颌骨扩张模式。
然而，没有可用的文献使用有限元分析 （FEA） 模型研究截骨术对 SARPE 后不对称性的影响。目前所有的研究都采用了对称截骨模式6,7,8,9,10,11,12,14的模型，这并不能反映临床实践的现实，即截骨术在颅骨的每一侧可能不同。缺乏研究不对称截骨术对 SARPE 后不对称影响的文献，这是一个必须解决的重大知识差距。
因此，本研究的目的是开发一种新的 SARPE FEA 模型，该模型可以真正模拟临床状况，包括扩张量和截骨间隙，并研究各种截骨设计下半上颌骨在三个维度的扩张模式。这种方法将为 SARPE 后扩增模式背后的机制提供有价值的见解，并作为临床医生规划和执行 SARPE 程序的有用工具。

<table border="1" fo:keep-together.within-page="1" fo:keep-with-next.within-page="always">
	<tbody>
		<tr>
			<td>Ansys</td>
			<td>Ansys</td>
			<td>Version 2019</td>
			<td>Ansys is a software for finite element analysis that can solve complicated models based on differential equations. The expansion results of different buccal osteotomy angles were analyzed through this software.</td>
		</tr>
		<tr>
			<td>Geomagic Studio</td>
			<td>3D Systems</td>
			<td>Version 10</td>
			<td>Geomagic Studio is a software for reverse engineering that can generate digital models based on physical scanning points. This study built cancellous bone and periodontal ligaments through this software.</td>
		</tr>
		<tr>
			<td>Mimics</td>
			<td>Materialise</td>
			<td>Version 16</td>
			<td>Mimics is a medical 3D image-based engineering software that efficiently converts CT images to a 3D model. This study reconstructed a maxilla complex through the patient&#39;s DICOM images.</td>
		</tr>
		<tr>
			<td>SolidWorks</td>
			<td>Dassault Syst&#232;mes</td>
			<td>Version 2018</td>
			<td>SolidWorks is a computer-aided design software for designers and engineers to create 3D models. A Haas expander was designed and drawn through this software in this study.</td>
		</tr>
	</tbody>
</table>

finite element analysis model for assessing expansion patterns from surgically assisted rapid palatal expansion

引入手术辅助快速腭扩张 （SARPE） 以释放骨阻力，以促进骨骼成熟患者的骨骼扩张。然而，据报道，在所有 SARPE 患者中，有 7.52% 的患者出现左右两侧不对称扩张，其中 12.90% 的患者必须接受第二次手术进行矫正。导致不对称扩张的病因尚不清楚。有限元分析已被用于评估颌面结构中与SARPE相关的应力。然而，由于LeFort I截骨部位的骨骼碰撞仅在一定程度的扩张后发生，因此大多数现有模型并不能真正代表力分布，因为这些现有模型的扩张量很少超过1 mm。因此，有必要创建一个新的SARPE有限元模型，该模型可以执行临床所需的扩张激活量，以进一步分析所有三个维度的半上颌骨扩张模式。将锥形束计算机断层扫描 （CBCT） 的三维 （3D） 颅骨模型导入 Mimics 并转换为数学实体，以分割上颌复合体、上颌第一前磨牙和上颌第一磨牙。这些结构被转移到Geomagic中，用于表面平滑和松质骨和牙周韧带的创建。然后保留上颌骨的右半部分并镜像，以在 SolidWorks 中创建完美对称的模型。构建了 Haas 扩张器并将其绑扎到上颌第一前磨牙和第一磨牙上。在Ansys中对不同角度、间隙为1 mm的各种颊切骨术组合进行了有限元分析。进行收敛测试，直到达到所需的两侧膨胀量（总共至少 6 毫米）。本研究为评估颊骨切开成角如何影响SARPE的扩张模式奠定了基础。

Surgically assisted rapid palatal expansion (SARPE) is a commonly used technique for transversely expanding the maxillary bony structure and the dental arch in skeletally mature patients1. The surgery involves a LeFort I osteotomy, a mid-palatal corticotomy, and, optionally, the release of the pterygoid-maxillary fissure2. However, undesired expansion patterns from SARPE, such as uneven expansion between left and right hemimaxillae3 and dentoalveolar process buccal tipping/rotation4, have been reported, which could lead to failure of SARPE, and sometimes, even requiring additional surgeries for correction5. Previous studies have indicated that the variation in circum-maxillary osteotomies may play a significant role in post-SARPE expansion pattern2,3, as the collisions between the bone blocks at the Le Fort I osteotomy sites can contribute to the uneven resisting force of lateral expansion of the hemimaxillae and to the rotation of the hemimaxillae with the alveolar edges below the cut moving inwards while the dentoalveolar process expands3,4. Therefore, there is a need to investigate the effects of different osteotomy directions, especially the buccal osteotomy, on post-SARPE expansion patterns.
Several finite element analysis (FEA) models have been set up to evaluate the force distribution during SARPE. However, the amount of expansion set in these models is limited to up to 1 mm, which is far below the required clinical amount6,7,8,9,10,11,12. Inadequate expansion in FEA models can lead to erroneous predictions of post-SARPE outcomes. More specifically, the collision between the bones at the osteotomy site, as reported by Chamberland and Proffit4, may not be demonstrated if the expander is not adequately turned, which may not reflect the true clinical reality. With the limited amount of expansion built in the previous models, the outcome evaluations of these models were focused on stress analysis. However, the stress analysis of FEA in dentistry is usually conducted under static loading with the mechanical properties of materials set as isotropic and linearly elastic, which further restricts the clinical relevance of the FEA studies13.
Furthermore, most of these studies did not consider the thickness of the surgical instrument at the osteotomy site6,7,8,10,11,12, often setting friction to zero at the cuts as part of the boundary conditions. However, this setting oversimplifies the contacts between the hard and soft tissues. It may significantly impact the distribution of force and the resulting expansion pattern of the hemimaxillae.
Nevertheless, no available literature has investigated the effect of osteotomy on post-SARPE asymmetry using finite element analysis (FEA) models. All the current studies employed models with symmetrical osteotomy patterns6,7,8,9,10,11,12,14, which do not reflect the reality of clinical practice where the osteotomies may differ on each side of the skull. The lack of literature examining the effect of asymmetrical osteotomies on post-SARPE asymmetry represents a significant knowledge gap that must be addressed.
Therefore, the goal of this study is to develop a novel FEA model of SARPE that can truly mimic the clinical conditions, including the expansion amount and osteotomy gap, and investigate the expansion patterns of the hemimaxillae in all three dimensions with various designs of the osteotomy. Such an approach would provide valuable insight into the mechanics underlying post-SARPE expansion patterns and serve as a useful tool for clinicians in the planning and execution of SARPE procedures.

作者聚焦：开发一种用于改进正颌手术技术的新型有限元分析模型 

用于评估手术辅助快速腭扩张模式的有限元分析模型

SARPE is commonly used for maxillary expansion in skeletal immature patients. However, asymmetric expansion has been reported with unknown etiologies. This study aims to develop a novel FEA model of SARPE that can truly mimic the clinical conditions, and to investigate the expansion patterns of the hemi-maxilla in all three dimensions.Finite element analysis has been used in the dental and bioengineering field to allow in vitro simulation of surgeries, such as SARPE. In this study, four software were utilized to set up the FEA model and to predict expansion pattern. The most challenging part, which most previous studies link, is to simulate forces at the wound healing site across osteotomy surface.To achieve this, springs were set in our pilot study and is considered a novel design for SARPE FEA. This unified element model focused on its patient patterns, making it more realistic SARPE simulation through osteotomy gap creation and experience inclusion. It presents significant potential as the clinical tool for branding and its guiding SARPE procedures.Our interdisciplinary group will work diligently to develop cutting-edge 3D models that can provide valuable insights into personalized treatment strategies to analyze and improve orthognatic surgical technique by utilizing an engineering-assisted approach and to improve communication and collaboration between orthodontists and oral maxillofacial surgeons through engineering-assisted 3D imaging system.

该演示模型利用了一名 47 岁患有上颌骨缺陷的女性的 CBCT 图像。在生成的模型中，保留了鼻腔、上颌窦和扩张锚定牙齿（第一前磨牙和第一磨牙）的牙周韧带空间的解剖结构（图 1）。
为了准确模拟手术过程，在所有模拟中，鼻中隔、鼻腔侧壁和翼上颌裂与上颌体分离。此外，还创建了一个代表手术期间颊口截骨术的平面，厚度为 1 毫米。该平面从梨?...

Watch this Scientific Journal Video about Development of a Novel Finite Element Analysis Model for Improved Orthognathic Surgical Techniques at JoVE.com

创建了一套新的手术辅助快速腭扩张 （SARPE） 有限元模型，该模型可以在不同角度的颊骨截骨术中执行临床所需的扩张器激活量，以进一步分析所有三个维度的半上颌骨扩张模式。

Surgically assisted rapid palatal expansion (SARPE) was introduced to release bony resistance to facilitate skeletal expansion in skeletally mature ...

SARPE 通常用于骨骼未成熟患者的上颌扩张。然而，已有不对称扩张的报道，病因不明。本研究旨在开发一种能够真正模拟临床状况的新型 SARPE 有限元分析模型，并研究半上颌骨在三个维度上的扩张模式。有限元分析已被用于牙科和生物工程领域，以实现手术的体外模拟，例如 SARPE。在这项研究中，使用了四个软件来建立有限元分析模型并预测膨胀模式。最具挑战性的部分，大多数以前的研究都与之相关，是模拟截骨术表面伤口愈合部位的力。为了实现这一目标，在我们的试点研究中设置了弹簧，并被认为是 SARPE FEA 的一种新颖设计。这个统一的元素模型专注于其患者模式，通过截骨术间隙创建和体验包容使其更加逼真。它作为品牌推广及其指导 SARPE 程序的临床工具具有巨大的潜力。我们的跨学科团队将努力开发尖端的 3D 模型，为个性化治疗策略提供有价值的见解，利用工程辅助方法分析和改进正颌外科技术，并通过工程辅助 3D 成像系统改善正畸医生和口腔颌面外科医生之间的沟通和协作。

finite-element-analysis-model-for-assessing-expansion-patterns-from

Research

JoVE Journal

Bioengineering

Finite Element Analysis Model for Assessing Expansion Patterns from Surgically Assisted Rapid Palatal Expansion

896 次观看.  University of Pennsylvania. SARPE 通常用于骨骼未成熟患者的上颌扩张。然而，已有不对称扩张的报道，病因不明。本研究旨在开发一种能够真正模拟临床状况的新型 SARPE 有限元分析模型，并研究半上颌骨在三个维度上的扩张模式。有限元分析已被用于牙科和生物工程领域，以实现手术的体外模拟，例如 SARPE。在这项研究中，使用了四个软件来建立有限元分析模型并预测膨胀模式。最具挑战性的部...

视频: 作者聚焦：开发一种用于改进正颌手术技术的新型有限元分析模型 

Surgically assisted rapid palatal expansion (SARPE) was introduced to release bony resistance to facilitate skeletal expansion in skeletally mature patients. However, asymmetric expansion between the left and right sides has been reported in 7.52% of all SARPE patients, of which 12.90% had to undergo a second surgery for correction. The etiologies leading to asymmetric expansion remain unclear. Finite element analysis has been used to evaluate the stress associated with SARPE in the maxillofacial structures. However, as a collision of the bone at the LeFort I osteotomy sites occurs only after a certain amount of expansion, most of the existing models do not truly represent the force distribution, given that the expansion amount of these existing models rarely exceeds 1 mm. Therefore, there is a need to create a novel finite element model of SARPE that could perform a clinically required amount of expander activation for further analysis of the expansion patterns of the hemimaxillae in all three dimensions. A three-dimensional (3D) skull model from cone beam computed tomography (CBCT) was imported into Mimics and converted into mathematical entities to segment the maxillary complex, maxillary first premolars, and maxillary first molars. These structures were transferred into Geomagic for surface smoothing and cancellous bone and periodontal ligament creation. The right half of the maxillary complex was then retained and mirrored to create a perfectly symmetrical model in SolidWorks. A Haas expander was constructed and banded to the maxillary first premolars and first molars. Finite element analysis of various combinations of buccal osteotomies at different angles with 1 mm clearance was performed in Ansys. A convergence test was conducted until the desired amount of expansion on both sides (at least 6 mm in total) was achieved. This study lays the foundation for evaluating how buccal osteotomy angulation influences the expansion patterns of SARPE.

A set of novel finite element models of surgically assisted rapid palatal expansion (SARPE) that could perform a clinically required amount of expander activation with various angles of buccal osteotomy was created for further analysis of the expansion patterns of the hemimaxillae in all three dimensions.

科研

生物工程

Finite Element Analysis Model: Osteotomy Design to Detect Palatal Expansion

To begin, launch the SolidWorks software to create a one-millimeter thick plane from the piriform aperture towards the infra-zygomatic crest. Now open the Insert menu, then click on Reference Geometry and Plane options. From the osteotomy plane, select three feature points and click OK to create the O1 plane.Navigate to the plane again by clicking on Insert and Reference Geometry. This time, choose the osteotomy plane and set an offset distance of one millimeter. Click OK to create a lower cutting plane marked O2.Now navigate to split by selecting Insert, followed by Features, and choose the O1 and O2 planes in Trim Tools.Select the target bodies and press Cut Bodies to create a cutting preview. Next, tick the check boxes in the Resulting Bodies section and press OK to separate the maxillary complex. Then click on the body between the O1 and O2 planes, right-click, and press Delete under the Body section.To export the models with different buccal osteotomy angles, first click on File, then Save As, and choose Parasolid x_t from the file type list. Finally, click Save to export the models for finite element analysis software. The demonstrated analysis used the cone-beam computed tomography image of a 47-year-old female with maxillary deficiency to generate a model.For accurate surgery simulation, the nasal septum, lateral nasal cavity walls, and pterygomaxillary fissure were separated.

有限元分析模型：截骨设计检测腭扩张

Expansion Assessment Using Finite Element Analysis from Surgically Assisted Rapid Palatal Expansion (SARPE)

To begin, launch the Ansys software to import the material parameters of the maxillary complex model into the software. Next, click and drag the static structural in the toolbox to create an analysis workspace. Double click on engineering data, followed by linear elastic under toolbox, and set the Young's modulus and Poisson's ratio for all the materials in properties.Now, double click on geometry, followed by file, then select import external geometry file, and click generate to import the maxillary complex model. Then click create, followed by Boolean, and generate the cortical and periodontal ligament Boolean with cancellous bone and teeth. To set up the finite element analysis model, double click on the model, then select geometry to determine the material properties for each part.Next, right click on mesh and press generate mesh to build the model elements. Now, click connections and assign the soft or small part in contact bodies, and the stiff or large part in target bodies, then assign the contact type and friction coefficient in definition. Next, right click connections and select insert, then press spring to connect the upper and lower parts of the osteotomy plane.Set the springs to one millimeter length with a spring constant K set at 60 newtons per millimeter. Place one spring at each grid node. After setting a clinically acceptable force along the X axis, right click the static structural option.Press insert, followed by fixed support to render the structure on the palatal plane as immovable. To apply force on the acrylic plate away from the medial line, click on static structural, then insert and set the force to 150 newtons. Then right click solution followed by insert, deformation, and total to monitor the expansion deformation.Finally, to carry out a convergence test, select solve in the toolbars and wait until the force convergence level reaches the force criterion. Then click on solution information, followed by total deformation to display the expansion results. The demonstrated model used the cone beam computed tomography image of a 47-year-old female with maxillary deficiency to create a model.For accurate surgery simulation, the naval septum, lateral nasal cavity walls, and pterygo-maxillary fissure were separated. A preliminary test performed on both the left and right sides of the model with symmetric, zero degree cuts, showed that 150 newtons of force caused more than eight millimeters of expansion. Additionally, a variety of angles were built to mimic different clinical conditions.The right and left expansions were visible as a before and after color map of the maxilla models.