The first author would like to acknowledge grants from the National Natural Science Foundation of China (No. 52078152 and No. 12002095), General Program of Guangzhou Science and Technology Plan (No. 202102021113), Guangzhou Government-University Union Fund (No. 202201020532), and&#160;Guangzhou Municipal Science and Technology Project (Grant No. 202102020606).

1. Creating the surface in the CAD software
<ol>
	<li>Open the CAD software (see Table of Materials), left-click on File, left-click on New, and select Part.</li>
	<li>In Part1, right-click on Top, and select Show.</li>
	<li>Create a new plane: Press Ctrl, and left-click to select the Top plane and drag it up. Enter 30 mm as the Offset Distance, and rename the plane &#34;Bottom&#34;.</li>
	<li>Create a sketch on the &#34;Top&#34; plane.
	<ol>
		<li>Right-click on Top, and select Sketch to create Sketch 1. Select Equation Driven Curve in Spline of the Sketch.</li>
		<li>Select Parametric in Equation Type. Input the parameters according to Table 1. 
		NOTE: The sketch shape of the top plane is generated in this step. For example, if one desires to create a CT, enter 7.21 x sin(t), 7.21 x cos(t), 0 and 2 x pi in Table 1 in this step.</li>
	</ol>
	</li>
	<li>Create a sketch on the &#34;Bottom&#34; plane.
	<ol>
		<li>Right-click on Bottom, and select Sketch to create Sketch 2. Select Equation Driven Curve in Spline.</li>
		<li>Select Parametric in Equation Type. Input the parameters according to Table 1. 
		NOTE: The sketch shape of the bottom plane is generated in this step. For example, if you want to create a CT, enter 12.5 x sin(t), 12.5 x cos(t), 0, and 2 x pi in Table 1 in this step.</li>
	</ol>
	</li>
	<li>Generate the surface.
	<ol>
		<li>Left-click on Lofted surface. Select Sketch 1 and Sketch 2 in Profiles, and select OK (see Supplementary File 1).</li>
	</ol>
	</li>
	<li>Repeat the above steps (steps 1.1-1.6) to generate three kinds of surfaces (Figure 1A), and name them CT, ST, and DT, as shown in Figure 1A. 
	NOTE: Step 1.4.4 and step 1.5.4 create the sketches of the top and bottom planes, respectively, and step 1.6 connects the sketches of the top and bottom planes together to form a surface. The difference between the three planes is in the sketch of step 1.4.4 and step 1.5.4.</li>
</ol>
2. Building the model in the finite element software
NOTE: The quasi-static compression model of ST with k = 0.9 is described here as an example. The finite element models of the three types of tubes are exactly the same. Therefore, the different types of tubes in step 2.1.1 are to be imported, and step 2 needs to be repeated to get all the results.
<ol>
	<li>Parts: Import and create the parts.
	<ol>
		<li>Open the finite element software (see Table of Materials). Import the part &#34;ST&#34;: left click File &#62; Import &#62; Part in order.Select the file ST, and name this part &#34;ST&#34; (see Supplementary File 2).</li>
		<li>Create the part &#34;Bottom Plane&#34;: Left-click on Create Part. Under Shape, select Shell, name this part &#34;Bottom Plane&#34;, and left-click on Continue. Select Create Circle: Center and Perimeter, and draw a circle with the origin as the center and a radius of 20 mm. Add the reference point set4 to the part &#34;Bottom Plane&#34;.</li>
		<li>Create the part &#34;Top Plane&#34;: Left-click on Create Part. Under Shape, select Shell, name this part &#34;Top Plane&#34;, and left-click on Continue. Select Create Circle: Center and Perimeter, and draw a circle with the origin as the center and a radius of 20 mm.Add the reference point set5 to the part &#34;Top Plane&#34;.</li>
	</ol>
	</li>
	<li>Property: Define the materialproperties, and assign the material to the section.
	<ol>
		<li>Create the material properties. 
		NOTE: The three types of tubes have the same material properties.
		<ol>
			<li>Left-click on Create Material &#62; General &#62; Density in order,and enter &#34;7.85E-09 (7.85 x 10&#8722;9)&#34; under &#34;Mass Density&#34;. 
			NOTE: The material properties are obtained from previously published reports41 with the same materials, and an introduction to the materials is included in the discussion section.</li>
			<li>Left-click on Mechanical &#62; Elasticity &#62; Elastic in order, and under Young&#39;s Modulus and Poisson&#39;s Ratio, input &#34;185,000&#34; and &#34;0.3&#34;, respectively.</li>
			<li>Left-click on Mechanical &#62; Plasticity &#62; Plastic in order, and enter the data taken from Figure 2 in &#34;Yield Stress&#34; and &#34;Plastic Strain&#34;.</li>
		</ol>
		</li>
		<li>Assign the section.
		<ol>
			<li>Left-click on Create Section, under &#34;Category&#34;, select Shell, and left-click on Continue.</li>
			<li>Under &#34;Shell Thickness&#34; select Nodal Distribution, left-click on Create Analytical Field, select Expression field, and enter the formula &#34;0.44 &#8722; 0.9/100 x (Y &#8722; 15)&#34;. 
			NOTE: The formula is used to change the thickness of the tube in the height direction and achieve the thickness gradient. The thickness variation factor k is defined as shown in Figure 1C, which indicates the thickness variation per unit height. In addition, the thickness of half of the height is set to a fixed value (i.e., th/2 = 0.44 mm) so that the thickness of the other heights can be derived from the middle height: 
			0.44&#160;&#8722; k/100 &#215; (Y &#8722; 15) 
			where Y is the height direction in the software.</li>
			<li>Left-click on Assign Section, pick ST from the interface, left-click on Done, and left-click on OK.</li>
		</ol>
		</li>
	</ol>
	</li>
	<li>Assembly: Assemble the parts into a whole.
	<ol>
		<li>Left-click on Create Instance, and&#160;select ST, Bottom Plane, and Top Plane. Then, left-click on OK&#160;|&#160;Rotate Instance, and select Bottom Plane and Top Plane. Enter the start point (0, 0, 0) and end point (1, 0, 0) of the rotation axis in turn, and enter 90 under Angle of Rotation. Left-click on Translate Instance, select Top Plane, and enter the start point (0, 0, 0) and end point (0, 30, 0) of the translation vector in turn.</li>
	</ol>
	</li>
	<li>Step: Create an analysis step, and set the history output items.
	<ol>
		<li>Left-click on Create Step, select Dynamic, Explicit, and left-click on Continue. Under Time Period enter 0.05, and left-click on OK. Left-click on Create History Output, and select Energy.</li>
		<li>Left-click on Create History Output; under &#34;Domain&#34; select Set5, under &#34;Output Variables&#34; enter &#34;RF2, U2&#34;, and left-click on OK.</li>
	</ol>
	</li>
	<li>Interaction: Set the contact properties and type, and set the top plane and bottom plane as rigid bodies.
	<ol>
		<li>Left-click on Create Interaction Property, and select Contact. Under &#34;Mechanical&#34; select Tangential Behavior, under &#34;Friction formulation&#34; select Penalty, and under &#34;Friction Coeff&#34; enter &#34;0.2&#34;.</li>
		<li>Left-click on Create Interaction, select General Contact (Explicit), and under &#34;Global property assignment&#34; select intProp-1.</li>
		<li>Left-click on Create Constraint, under &#34;Type&#34; select Rigid body, and pick up Bottom Plane and Top Plane.</li>
	</ol>
	</li>
	<li>Load: Fix the bottom plane, and set a downward loading speed of 500 mm/s on the top plane.
	<ol>
		<li>Left-click on Create Boundary Condition, under &#34;Types for Selected Step&#34; select Displacement/Rotation, pick up set4, and enter 0 in all directions .</li>
		<li>Left-click on Create Boundary Condition, under &#34;Types for Selected Step&#34; select Velocity/Angular Velocity, pick up set5, enter &#8722;500 under &#34;V2&#34;, and enter 0 in the other direction.</li>
	</ol>
	</li>
	<li>Mesh: Meshing and determining the element types. 
	NOTE: Step 2.7 is important in the finite element analysis. The structure meshes into a finite number of elements, a suitable mathematical approximation solution is assumed for each element, and then the equilibrium conditions for the whole structure are derived and solved to obtain the solution to the problem.
	<ol>
		<li>Left-click on Seed Part, enter 0.8 under &#34;Approximate Global Size&#34;, and enter 0.08 under &#34;By Absolute Value&#34;. Left-click on Mesh Part, and select Yes.</li>
		<li>Left-click on Assign Element Type, pick up the part, and select Done. Under &#34;Element Library&#34; select Explicit, and left-click on OK.</li>
		<li>Repeat step 2.7 to mesh the three parts CT, ST, and DT.The finite element model of the ST is shown in Figure 3.</li>
	</ol>
	</li>
	<li>Job: Submit the calculations, and export the results.
	<ol>
		<li>Left-click on Create Job, select the model to calculate, and left-click on Continue. Left-click on Job Manager, select the model to calculate, and left-click on Submit.</li>
		<li>Select the completed model for calculation, and left-click on Results to enter the Visualization. The deformation mode of the ST (k = 0.9) is obtained from the Visualization. Left-click on Create XY Date. Select ODB history output, and click on Plot to plot the force-displacement curve of the ST (k = 0.9).</li>
	</ol>
	</li>
	<li>In step 2, step 2.1.1 has three structural choices, and step 2.2.2.2 has six choices of thickness variation factor (k), while the other steps are the same. Therefore, repeat the above steps 18 times to obtain the deformation modes and force-displacement curves for 18 models, as shown in Figure&#160;4, Figure 5, Figure 6, Figure 7, Figure 8. In addition, the crashworthiness evaluation indicators are obtained from the force-displacement curve through Equations 1-4, as shown in Figure&#160;9, Figure 10, Figure 11 and Table 2. 
	NOTE: The introduction of the crashworthiness evaluation indicators and Equations 1-4 are in the representative results.</li>
</ol>

The authors have nothing to disclose.

The quasi-static compression performance of tapered tubes was studied by finite element analysis. Two new types of corrugated tapered tubes with variable thicknesses were designed, and their quasi-static compression performance was investigated. In quasi-static compression simulations, some important steps and settings need to be verified.
The material parameters are the basic requirements for the finite element calculation (step 2.2.1 of the protocol). In this study, the material parameters w...

Crashworthiness is an essential issue for lightweight automobiles, and thin-walled structures are widely used to improve crashworthiness. Typical thin-walled structures, such as round tubes, have good energy absorption capacity but usually have large peak forces and load fluctuations during the crushing process. This problem can be solved by introducing axial corrugations1,2,3. The presence of corrugations allows the tube to plastically deform and fold according to a predesigned corrugation pattern, which can reduce the peak force and load fluctuations4,5. However, this stable and controlled deformation pattern has a drawback: the energy absorption performance decreases. To improve the energy absorption of axial corrugated tubes, researchers have tried many methods, such as using a functional gradient design in the wavelength6,7 and amplitude8, using filling foam9,10, forming multichamber and multiwall structures11, and forming combined tubes12.
In addition, researchers have designed lateral corrugated tubes by introducing corrugations into the cross-section of circular tubes13,14,15,16. The existence of lateral corrugations greatly improves the energy absorption performance of the tube17,18,19. Eyvazian et al.20 compared the crashworthiness of lateral corrugated tubes and ordinary circular tubes and showed that lateral corrugated tubes had a better energy absorption capacity. One reason for this observation is that the lateral corrugation strengthens the tube wall, which makes it more resistant to plastic folding.&#160;In addition, the corrugated wall of the plastic folding part flattens, and this flattening also absorbs energy. However, the high initial peak force is a disadvantage of this type of tube, and this high initial force may seriously affect the safety of the passengers being transported.
Functionally graded structures have a natural advantage in reducing the peak force. Common functionally graded thin-walled tubes are usually formed by changing the geometric parameters (e.g., the diameter and wall thickness)21. The most prevalent structures for which the diameter is changed are tapered tubes, including circular tapered tubes22, square tapered tubes23,24,25, polygonal tapered tubes26,27, axial corrugated tapered tubes28,29,30, and tapered tubes with elliptical cross sections31. However, there are few studies on lateral corrugated tubes. Typical thickness gradient structures include square tubes32,33, circular tubes34,35, tapered tubes36, multicellular tubes37,38, and lattice structures39. Deng et al.40 reduced the initial peak force of lateral corrugated tubes with a thickness gradient design by 44.53%, but there have been no studies on lateral corrugated tapered tubes.
Although experiments are the most accurate and direct method to evaluate the crashworthiness of structures, they also require considerable money and resources. In addition, some important data, such as the stress-strain clouds of the structure and the energy values of different forms, are difficult to obtain in experiments18. Finite element analysis is a method to simulate the real load conditions by using mathematical approximation. This was first applied in the aerospace field, mainly for solving linear structural problems. Later, it was gradually applied to solve nonlinear problems in many fields, such as civil engineering, mechanical engineering, and material processing34.&#160;In addition, with finite element software development, simulation results have become increasingly close to those of the corresponding experiments. Therefore, simulation using finite element analysis is used to investigate the crashworthiness of the structures. In this study, finite element analysis of the quasi-static compression performance of corrugated tapered tubes was conducted. The energy absorption of two types of lateral corrugated tapered tubes (i.e., the single corrugated tapered tube [ST] and the double corrugated tapered tube [DT]) with variable thicknesses was studied numerically. The results were compared with those obtained for a conventional conical tube (CT).&#160;The dimensions of the three types of thin-walled tubes are shown in Figure 1A. The geometric parameters of the ST are shown in Figure 1B, and the DT is built by crossing two STs. The thickness gradient is designed as shown in Figure&#160;1C, and the thickness variation is defined by introducing a variation: factor k. In Figure&#160;1C, th/2 = 0.44 mm, and k is set to 0, 0.3, 0.6, 0.9, 1.2, and 1.5. The results show that the peak crushing force decreases and the crushing force efficiency increases with increases in k.

<table><tbody><tr><td>ABAQUS</td><td>Dassault SIMULIA</td><td>Finite element software</td><td></td></tr><tr><td>CT</td><td>Botong 3D printing</td><td>Conical tube for experiment</td><td></td></tr><tr><td>SOLIDWORKS</td><td>Dassault Systemes</td><td>CAD software</td><td></td></tr><tr><td>Universal testing machine</td><td>SUNS</td><td>UTM5205, 200kN</td><td></td></tr></tbody></table>

finite element modeling for the simulation of the quasi-static compression of corrugated tapered tubes

In this study, the quasi-static compression performance of tapered tubes was investigated using finite element simulations. Previous studies have shown that a thickness gradient can reduce the initial peak force and that lateral corrugation can increase the energy absorption performance. Therefore, two kinds of lateral corrugated tapered tubes with variable thicknesses were designed, and their deformation patterns, load displacement curves, and energy absorption performance were analyzed. The results showed that when the thickness variation factor (k) was 0.9, 1.2, and 1.5, the deformation mode of the single corrugated tapered tube (ST) changed from transverse expansion and contraction to axial progressive folding. In addition, the thickness gradient design improved the energy absorption performance of the ST. The energy absorption (EA) and specific energy absorption (SEA) of the model with k = 1.5 increased by 53.6% and 52.4%, respectively, compared with the ST model with k = 0. The EA and SEA of the double corrugated tapered tube (DT) increased by 373% and 95.7%, respectively, compared with the conical tube. The increase in the k value resulted in a significant decrease in the peak crushing force of the tubes and an increase in the crushing force efficiency.

Several commonly used indicators are used to determine the crashworthiness of structures, including the total energy absorption (EA), specific energy absorption (SEA), peak crushing force (PCF), mean crushing force (MCF), and crushing force efficiency (CFE)42.
The total energy absorption (EA)43 can be expressed as follows:
<img alt="Equation 1" src="/files/ftp_upload/64708/64708eq01.jpg" style="margin: auto;" />&#160; ...

Read this Scientific Article Protocol about Finite Element Modeling for the Simulation of the Quasi-Static Compression of Corrugated Tapered Tubes at JoVE.com

Finite Element Modeling for the Simulation of the Quasi-Static Compression of Corrugated Tapered Tubes

This protocol describes the study of the quasi-static compression performance of corrugated tapered tubes using finite element simulations. The influence of the thickness gradient on the compression performance was investigated. The results show that proper thickness gradient design can change the deformation mode and significantly improve the energy absorption performance of the tubes.

In this study, the quasi-static compression performance of tapered tubes was investigated using finite element simulations. Previous studies have shown ...

finite-element-modeling-for-simulation-quasi-static-compression

Universidad de Cartagena UDEC

Research

JoVE Journal

Engineering

1.6K Views.  Guangzhou University. This protocol describes the study of the quasi-static compression performance of corrugated tapered tubes using finite element simulations. The influence of the thickness gradient on the compression performance was investigated. The results show that proper thickness gradient design can change the deformation mode and significantly improve the energy absorption performance of the tubes.

Video: Finite Element Modeling for the Simulation of the Quasi-Static Compression of Corrugated Tapered Tubes

Experimental Methods for Investigation of Shape Memory Based Elastocaloric Cooling Processes and Model Validation

Shape Memory Alloys (SMA) using elastocaloric cooling processes have the potential to be an environmentally friendly alternative to the conventional vapor compression based cooling process. Nickel-Titanium (Ni-Ti) based alloy systems, especially, show large elastocaloric effects. Furthermore, exhibit large latent heats which is a necessary material property for the development of an efficient solid-state based cooling process. A scientific test rig has been designed to investigate these processes and the elastocaloric effects in SMAs. The realized test rig enables independent control of an SMA&#39;s mechanical loading and unloading cycles, as well as conductive heat transfer between SMA cooling elements and a heat source/sink. The test rig is equipped with a comprehensive monitoring system capable of synchronized measurements of mechanical and thermal parameters. In addition to determining the process-dependent mechanical work, the system also enables measurement of thermal caloric aspects of the elastocaloric cooling effect through use of a high-performance infrared camera. This combination is of particular interest, because it allows illustrations of localization and rate effects &#8212; both important for efficient heat transfer from the medium to be cooled.
The work presented describes an experimental method to identify elastocaloric material properties in different materials and sample geometries. Furthermore, the test rig is used to investigate different cooling process variations. The introduced analysis methods enable a differentiated consideration of material, process and related boundary condition influences on the process efficiency. The comparison of the experimental data with the simulation results (of a thermomechanically coupled finite element model) allows for better understanding of the underlying physics of the elastocaloric effect. In addition, the experimental results, as well as the findings based on the simulation results, are used to improve the material properties.

Experimental methods for investigation of solid state cooling processes and characterization of elastocaloric material properties of Shape Memory Alloys (SMA) are presented. A custom-built test rig has been designed for controlling and comprehensive monitoring of elastocaloric cooling processes. Furthermore, it provides a validation platform for thermomechanically coupled modeling approaches.

Shape Memory Alloys (SMA) using elastocaloric cooling processes have the potential to be an environmentally friendly alternative to the conventional vapor ...

Knowledge Based Cloud FE Simulation of Sheet Metal Forming Processes

The use of Finite Element (FE) simulation software to adequately predict the outcome of sheet metal forming processes is crucial to enhancing the efficiency and lowering the development time of such processes, whilst reducing costs involved in trial-and-error prototyping. Recent focus on the substitution of steel components with aluminum alloy alternatives in the automotive and aerospace sectors has increased the need to simulate the forming behavior of such alloys for ever more complex component geometries. However these alloys, and in particular their high strength variants, exhibit limited formability at room temperature, and high temperature manufacturing technologies have been developed to form them. Consequently, advanced constitutive models are required to reflect the associated temperature and strain rate effects. Simulating such behavior is computationally very expensive using conventional FE simulation techniques.
This paper presents a novel Knowledge Based Cloud FE (KBC-FE) simulation technique that combines advanced material and friction models with conventional FE simulations in an efficient manner thus enhancing the capability of commercial simulation software packages. The application of these methods is demonstrated through two example case studies, namely: the prediction of a material's forming limit under hot stamping conditions, and the tool life prediction under multi-cycle loading conditions.

The following paper presents a novel FE simulation technique (KBC-FE), which reduces computational cost by performing simulations on a cloud computing environment, through the application of individual modules. Moreover, it establishes a seamless collaborative network between world leading scientists, enabling the integration of cutting edge knowledge modules into FE simulations.

The use of Finite Element (FE) simulation software to adequately predict the outcome of sheet metal forming processes is crucial to enhancing the ...

A Coupled Experiment-finite Element Modeling Methodology for Assessing High Strain Rate Mechanical Response of Soft Biomaterials

This study offers a combined experimental and finite element (FE) simulation approach for examining the mechanical behavior of soft biomaterials (e.g. brain, liver, tendon, fat, etc.) when exposed to high strain rates. This study utilized a Split-Hopkinson Pressure Bar (SHPB) to generate strain rates of 100-1,500 sec-1. The SHPB employed a striker bar consisting of a viscoelastic material (polycarbonate). A sample of the biomaterial was obtained shortly postmortem and prepared for SHPB testing. The specimen was interposed between the incident and transmitted bars, and the pneumatic components of the SHPB were activated to drive the striker bar toward the incident bar. The resulting impact generated a compressive stress wave (i.e. incident wave) that traveled through the incident bar. When the compressive stress wave reached the end of the incident bar, a portion continued forward through the sample and transmitted bar (i.e. transmitted wave) while another portion reversed through the incident bar as a tensile wave (i.e. reflected wave). These waves were measured using strain gages mounted on the incident and transmitted bars. The true stress-strain behavior of the sample was determined from equations based on wave propagation and dynamic force equilibrium. The experimental stress-strain response was three dimensional in nature because the specimen bulged. As such, the hydrostatic stress (first invariant) was used to generate the stress-strain response. In order to extract the uniaxial (one-dimensional) mechanical response of the tissue, an iterative coupled optimization was performed using experimental results and Finite Element Analysis (FEA), which contained an Internal State Variable (ISV) material model used for the tissue. The ISV material model used in the FE simulations of the experimental setup was iteratively calibrated (i.e. optimized) to the experimental data such that the experiment and FEA strain gage values and first invariant of stresses were in good agreement.

The current study prescribes a coupled experiment-finite element simulation methodology to obtain the uniaxial dynamic mechanical response of soft biomaterials (brain, liver, tendon, fat, etc.). The multiaxial experimental results that arose because of specimen bulging obtained from Split-Hopkinson Pressure Bar testing were rendered to a uniaxial true stress-strain behavior when simulated through iterative optimization of the finite element analysis of the biomaterial.

This study offers a combined experimental and finite element (FE) simulation approach for examining the mechanical behavior of soft biomaterials (e.g. ...

Bioengineering

Structural Design and Manufacturing of a Cruiser Class Solar Vehicle

Cruisers are multi-occupant solar vehicles that are conceived to compete in long-range (over 3,000 km) solar races based on the best compromise between the energy consumption and the payload. They must comply to the race&#39;s rules regarding the overall dimensions, the solar panel size, functionality, and safety and structural requirements, while the shape, the materials, the powertrain, and the mechanics are considered at the discretion of the designer. In this work, the most relevant aspects of the structural design process of a full-carbon fiber-reinforced plastic solar vehicle are detailed. In particular, the protocols used for the design of the lamination sequence of the chassis, the leaf springs structural analysis, and the crash test numerical simulation of the vehicle, including the safety cage, are described. The complexity of the design methodology of fiber-reinforced composite structures is compensated by the possibility of tailoring their mechanical characteristics and optimizing the overall weight of the car.

In this work, several aspects related to the structural design process of a full-carbon fiber-reinforced plastic solar vehicle are detailed, focusing on the monocoque chassis, the leaf springs, and the vehicle as a whole during a crash test.

Cruisers are multi-occupant solar vehicles that are conceived to compete in long-range (over 3,000 km) solar races based on the best compromise between ...

Design and Optimization Strategies of a High-Performance Vented Box

This study aims to solve the problems of air flow chaos and poor performance in a vented box caused by the heterogeneous distribution of airflow through the design of the internal structure of the vented box with constant energy consumption. The final goal is to evenly distribute the airflow inside the vented box. Sensitivity analysis was performed for three structural parameters: the number of pipes, the number of holes in the middle pipe, and the number of each increment from the inside to the outside pipe. A total of 16 random array sets of three structural parameters with four levels were determined using the orthogonal experimental design. Commercial software was used for the construction of a 3D model for the selected experimental points, and this data was used to obtain the airflow velocities, which were then used to obtain the standard deviation of each experimental point. According to the range analysis, the combination of the three structural parameters was optimized. In other words, an efficient and economical optimization method considering the performance of the vented box was established, and it could be widely used to extend the storage time of fresh food.

Here, we present the range analysis method to optimize the sample points generated by an orthogonal experimental design to ensure that fresh food can be stored in a vented box for a long time by regulating the airflow pattern.

This study aims to solve the problems of air flow chaos and poor performance in a vented box caused by the heterogeneous distribution of airflow through ...

 IVUS-Based Computational Method to Quantify Coronary Mechanical Properties

Intravascular Ultrasound Image-Based Finite Element Modeling Approach for Quantifying In Vivo Mechanical Properties of Human Coronary Artery

Quantifying the mechanical properties of coronary arterial walls could provide meaningful information for the diagnosis, management, and treatment of coronary artery diseases. Since patient-specific coronary samples are not available for patients requiring continuous monitoring, direct experimental testing of vessel material properties becomes impossible. Current coronary models typically use material parameters from available literature, leading to significant mechanical stress/strain calculation errors. Here, we would introduce a finite element model-based updating approach (FEMBUA) to quantify patient-specific in vivo material properties of coronary arteries based on medical images. In vivo cine intravascular ultrasound (IVUS) and virtual histology (VH)-IVUS images of coronary arteries were acquired from a patient with coronary artery disease. Cine IVUS images showing the vascular movement over one cardiac cycle were segmented, and two IVUS frames with maximum and minimum lumen circumferences were selected to represent the coronary geometry under systolic and diastolic pressure conditions, respectively. VH-IVUS image was also segmented to obtain the vessel contours, and a layer thickness of 0.05 cm was added to the VH-IVUS contours to reconstruct the coronary geometry. A computational finite element model was created with an anisotropic Mooney-Rivlin material model used to describe the vessel's mechanical properties and pulsatile blood pressure conditions prescribed to the coronary luminal surface to make it contract and expand. Then, an iterative updating approach was employed to determine the material parameters of the anisotropic Mooney-Rivlin model by matching minimum and maximum lumen circumferences from the computational finite element model with those from cine IVUS images. This image-based finite element model-based updating approach could be successfully extended to determine the material properties of arterial walls in various vascular beds and holds the potential for risk assessment of cardiovascular diseases.

In vivo cine intravascular ultrasound images show the coronary cross-sectional movement corresponding to different pressure loading conditions. Based on a finite element model, an iterative scheme was employed to determine the patient-specific mechanical properties of coronary arteries in vivo by matching coronary motion from the computational model and medical images.

Quantifying the mechanical properties of coronary arterial walls could provide meaningful information for the diagnosis, management, and treatment of ...

Surrogate Model Development for Digital Experiments in Welding

The manufacturing industry heavily relies on welding processes to join materials, forming integral components across various sectors. Many aspects will influence the quality of the weld and finally affect the structure integrity of the weldment. Welding-induced residual stress, a consequence of the thermal cycling inherent in these processes, significantly impacts the structural integrity and performance of fabricated components. Understanding and predicting this residual stress is crucial for enhancing the reliability and durability of welded structures. However, quickly assessing a welding setup in digital experiments presents significant challenges, as a traditional simulation may be time-consuming. This research outlines the application of a workflow to construct an artificial neural network-based surrogate model to predict welding-induced residual stress. The model is built using data automatically generated from finite element simulations through Python scripts based on macro functions. Unlike traditional methods that rely on manual preprocessing and finite element simulations, this approach significantly reduces the time and effort required for simulation setup and data extraction, enhancing overall efficiency. By ensuring that all simulation steps are performed consistently through macro functions, the method eliminates human-induced variability, leading to improved reproducibility. Furthermore, the automation of data generation makes it possible to create extensive datasets necessary for training machine learning models, overcoming the limitations of labor-intensive traditional techniques. The workflow contains four main steps: build a standard weld finite element simulation and validate the finite element simulation results against experimental data; develop scripts for large dataset generation using a macro function that records the preprocessing and postprocessing steps of the finite element simulation; use the scripts to generate the required data; develop surrogate models and test their performance. The artificial neural network demonstrated high accuracy in predicting stress levels, closely aligning with simulation results on the test dataset and a relative root mean square error of 0.0024.

This protocol outlines a general workflow for constructing an artificial neural network for welding simulation using datasets generated automatically through Python scripts with macro functions. The workflow is validated against a benchmark case involving single-pass, straight-line welding. The surrogate model's predictive accuracy shows a strong agreement with finite element simulations.

The manufacturing industry heavily relies on welding processes to join materials, forming integral components across various sectors. Many aspects will ...

Optical Coherence Tomography Based Biomechanical Fluid-Structure Interaction Analysis of Coronary Atherosclerosis Progression

In this paper, we present a complete workflow for the biomechanical analysis of atherosclerotic plaque in the coronary vasculature. With atherosclerosis as one of the leading causes of global death, morbidity and economic burden, novel ways of analyzing and predicting its progression are needed. One such computational method is the use of fluid-structure interaction (FSI) to analyze the interaction between the blood flow and artery/plaque domains. Coupled with in vivo imaging, this approach could be tailored to each patient, assisting in differentiating between stable and unstable plaques. We outline the three-dimensional reconstruction process, making use of intravascular Optical Coherence Tomography (OCT) and invasive coronary angiography (ICA). The extraction of boundary conditions for the simulation, including replicating the three-dimensional motion of the artery, is discussed before the setup and analysis is conducted in a commercial finite element solver. The procedure for describing the highly nonlinear hyperelastic properties of the artery wall and the pulsatile blood velocity/pressure is outlined along with setting up the system coupling between the two domains. We demonstrate the procedure by analyzing a non-culprit, mildly stenotic, lipid-rich plaque in a patient following myocardial infarction. Established and emerging markers related to atherosclerotic plaque progression, such as wall shear stress and local normalized helicity, respectively, are discussed and related to the structural response in the artery wall and plaque. Finally, we translate the results to potential clinical relevance, discuss limitations, and outline areas for further development. The method described in this paper shows promise for aiding in the determination of sites at risk of atherosclerotic progression and, hence, could assist in managing the significant death, morbidity, and economic burden of atherosclerosis.

There is a need to determine which atherosclerotic lesions will progress in the coronary vasculature to guide intervention before myocardial infarction occurs. This article outlines the biomechanical modeling of arteries from Optical Coherence Tomography using fluid-structure interaction techniques in a commercial finite element solver to help predict this progression.

In this paper, we present a complete workflow for the biomechanical analysis of atherosclerotic plaque in the coronary vasculature. With atherosclerosis ...

Piping Networks and Pressure Losses

Source: Alexander S Rattner, Department of Mechanical and Nuclear Engineering, The Pennsylvania State University, University Park, PA
This experiment introduces the measurement and modeling of pressure losses in piping networks and internal flow systems. In such systems, frictional flow resistance from channel walls, fittings, and obstructions causes mechanical energy in the form of fluid pressure to be converted to heat. Engineering analyses are needed to size flow hardware to ensure acceptable frictional pressure losses and select pumps that meet pressure drop requirements.
In this experiment, a piping network is constructed with common flow features: straight lengths of tubing, helical tube coils, and elbow fittings (sharp 90&#176; bends). Pressure loss measurements are collected across each set of components using manometers - simple devices that measure fluid pressure by the liquid level in an open vertical column. Resulting pressure loss curves are compared with predictions from internal flow models.

Pressure Losses in Piping Networks and Internal Flow Systems

Source: Alexander S Rattner, Department of Mechanical and Nuclear Engineering, The Pennsylvania State University, University Park, PA
This experiment ...

Education

JoVE Science Education

Mechanical Engineering

Stresses under Combined Loadings

When analyzing a bent tube with a circular cross-section subjected to multiple forces, it is crucial to determine the stress distribution in order to maintain structural integrity under varied load conditions.
The process begins by slicing the tube at critical points and analyzing the internal forces and stress components at these sections, focusing on the centroid. Normal stresses, generated by axial forces and bending moments, are either compressive or tensile and vary across the section from the neutral axis to the outer edges.
Shearing stresses, which act tangentially to the section, arise from shear forces and torsional or twisting moments. These stresses provide insights into the overall stress state within the tube. In addition, the calculated stresses are combined to identify the principal stresses at specific points, which are the maximum and minimum normal stresses without shear components.
<img alt="Equation 1" src="/files/ftp_upload/15665/15665_Equation_1.svg" style="text-align: center; height: 40px;" />
From these, the maximum shearing stress is determined, a crucial factor in assessing the potential for failure.
<img alt="Equation 2" src="/files/ftp_upload/15665/15665_Equation_2.svg" style="text-align: center; height: 40px;" />
Saint-Venant&#39;s principle allows for the assumption that stresses become uniformly distributed in sections far from the points of load application. This principle allows the use of superposition to combine effects from different loads, provided the stresses remain within the material&#39;s proportional limits. This method ensures accurate predictions of how structural components behave under real-world conditions.

A bent tube with a circular cross-section subjected to several forces will produce stresses at certain points.
Calculating stresses involves passing a ...