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 border="1" fo:keep-together.within-page="1" fo:keep-with-next.within-page="always">
	<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

Research

JoVE Journal

Engineering

1.5K 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

Simulation, Fabrication and Characterization of THz Metamaterial Absorbers

Metamaterials (MM), artificial materials engineered to have properties that may not be found in nature, have been widely explored since the first theoretical1 and experimental demonstration2 of their unique properties. MMs can provide a highly controllable electromagnetic response, and to date have been demonstrated in every technologically relevant spectral range including the optical3, near IR4, mid IR5 , THz6 , mm-wave7 , microwave8 and radio9 bands. Applications include perfect lenses10, sensors11, telecommunications12, invisibility cloaks13 and filters14,15. We have recently developed single band16, dual band17 and broadband18 THz metamaterial absorber devices capable of greater than 80% absorption at the resonance peak. The concept of a MM absorber is especially important at THz frequencies where it is difficult to find strong frequency selective THz absorbers19. In our MM absorber the THz radiation is absorbed in a thickness of ~ &lambda;/20, overcoming the thickness limitation of traditional quarter wavelength absorbers. MM absorbers naturally lend themselves to THz detection applications, such as thermal sensors, and if integrated with suitable THz sources (e.g. QCLs), could lead to compact, highly sensitive, low cost, real time THz imaging systems.

This protocol outlines the simulation, fabrication and characterization of THz metamaterial absorbers. Such absorbers, when coupled with an appropriate sensor, have applications in THz imaging and spectroscopy.

Metamaterials (MM),  artificial materials engineered to have properties that may not be found in  nature, have been widely explored since the first ...

Monolayer Contact Doping of Silicon Surfaces and Nanowires Using Organophosphorus Compounds

Monolayer Contact Doping (MLCD) is a simple method for doping of surfaces and nanostructures1. MLCD results in the formation of highly controlled, ultra shallow and sharp doping profiles at the nanometer scale. In MLCD process the dopant source is a monolayer containing dopant atoms.
In this article a detailed procedure for surface doping of silicon substrate as well as silicon nanowires is demonstrated. Phosphorus dopant source was formed using tetraethyl methylenediphosphonate monolayer on a silicon substrate. This monolayer containing substrate was brought to contact with a pristine intrinsic silicon target substrate and annealed while in contact. Sheet resistance of the target substrate was measured using 4 point probe. Intrinsic silicon nanowires were synthesized by chemical vapor deposition (CVD) process using a vapor-liquid-solid (VLS) mechanism; gold nanoparticles were used as catalyst for nanowire growth. The nanowires were suspended in ethanol by mild sonication. This suspension was used to dropcast the nanowires on silicon substrate with a silicon nitride dielectric top layer. These nanowires were doped with phosphorus in similar manner as used for the intrinsic silicon wafer. Standard photolithography process was used to fabricate metal electrodes for the formation of nanowire based field effect transistor (NW-FET). The electrical properties of a representative nanowire device were measured by a semiconductor device analyzer and a probe station.

A detailed procedure for surface doping of Silicon interfaces is provided. The ultra-shallow surface doping is demonstrated by using phosphorus containing monolayers and rapid annealing process. The method can be used for doping of macroscopic area surfaces as well as nanostructures.

Monolayer Contact Doping (MLCD) is a simple method for doping of surfaces and nanostructures1. MLCD results in the formation of highly controlled, ultra ...

Simulation of the Planetary Interior Differentiation Processes in the Laboratory

A planetary interior is under high-pressure and high-temperature conditions and it has a layered structure. There are two important processes that led to that layered structure, (1) percolation of liquid metal in a solid silicate matrix by planet differentiation, and (2) inner core crystallization by subsequent planet cooling. We conduct high-pressure and high-temperature experiments to simulate both processes in the laboratory. Formation of percolative planetary core depends on the efficiency of melt percolation, which is controlled by the dihedral (wetting) angle. The percolation simulation includes heating the sample at high pressure to a target temperature at which iron-sulfur alloy is molten while the silicate remains solid, and then determining the true dihedral angle to evaluate the style of liquid migration in a crystalline matrix by 3D visualization. The 3D volume rendering is achieved by slicing the recovered sample with a focused ion beam (FIB) and taking SEM image of each slice with a FIB/SEM crossbeam instrument. The second set of experiments is designed to understand the inner core crystallization and element distribution between the liquid outer core and solid inner core by determining the melting temperature and element partitioning at high pressure. The melting experiments are conducted in the multi-anvil apparatus up to 27 GPa and extended to higher pressure in the diamond-anvil cell with laser-heating. We have developed techniques to recover small heated samples by precision FIB milling and obtain high-resolution images of the laser-heated spot that show melting texture at high pressure. By analyzing the chemical compositions of the coexisting liquid and solid phases, we precisely determine the liquidus curve, providing necessary data to understand the inner core crystallization process.

The high-pressure and high-temperature experiments described here mimic planet interior differentiation processes. The processes are visualized and better understood by high-resolution 3D imaging and quantitative chemical analysis.

A planetary interior is under high-pressure and high-temperature conditions and it has a layered structure. There are two important processes that led to ...

Laboratory Drop Towers for the Experimental Simulation of Dust-aggregate Collisions in the Early Solar System

For the purpose of investigating the evolution of dust aggregates in the early Solar System, we developed two vacuum drop towers in which fragile dust aggregates with sizes up to ~10 cm and porosities up to 70% can be collided. One of the drop towers is primarily used for very low impact speeds down to below 0.01 m/sec and makes use of a double release mechanism. Collisions are recorded in stereo-view by two high-speed cameras, which fall along the glass vacuum tube in the center-of-mass frame of the two dust aggregates. The other free-fall tower makes use of an electromagnetic accelerator that is capable of gently accelerating dust aggregates to up to 5 m/sec. In combination with the release of another dust aggregate to free fall, collision speeds up to ~10 m/sec can be achieved. Here, two fixed high-speed cameras record the collision events. In both drop towers, the dust aggregates are in free fall during the collision so that they are weightless and match the conditions in the early Solar System.

We present a technique to achieve low-velocity to intermediate-velocity collisions between fragile dust aggregates in the laboratory. For this purpose, two vacuum drop-tower setups have been developed that allow collision velocities between &#60;0.01 and ~10 m/sec. The collision events are recorded by high-speed imaging.

For the purpose of investigating the evolution of dust aggregates in the early Solar System, we developed two vacuum drop towers in which fragile dust ...

Fabrication of High Contrast Gratings for the Spectrum Splitting Dispersive Element in a Concentrated Photovoltaic System

High contrast gratings are designed and fabricated and its application is proposed in a parallel spectrum splitting dispersive element that can improve the solar conversion efficiency of a concentrated photovoltaic system. The proposed system will also lower the solar cell cost in the concentrated photovoltaic system by replacing the expensive tandem solar cells with the cost-effective single junction solar cells. The structures and the parameters of high contrast gratings for the dispersive elements were numerically optimized. The large-area fabrication of high contrast gratings was experimentally demonstrated using nanoimprint lithography and dry etching. The quality of grating material and the performance of the fabricated device were both experimentally characterized. By analyzing the measurement results, the possible side effects from the fabrication processes are discussed and several methods that have the potential to improve the fabrication processes are proposed, which can help to increase the optical efficiency of the fabricated devices.

The fabrication of high contrast gratings as the parallel spectrum splitting dispersive element in a concentrated photovoltaic system is demonstrated. Fabrication processes including nanoimprint lithography, TiO2 sputtering and reactive ion etching are described. Reflectance measurement results are used to characterize the optical performance.

High contrast gratings are designed and fabricated and its application is proposed in a parallel spectrum splitting dispersive element that can improve ...

Simulation of Human-induced Vibrations Based on the Characterized In-field Pedestrian Behavior

For slender and lightweight structures, vibration serviceability is a matter of growing concern, often constituting the critical design requirement. With designs governed by the dynamic performance under human-induced loads, a strong demand exists for the verification and refinement of currently available load models. The present contribution uses a 3D inertial motion tracking technique for the characterization of the in-field pedestrian behavior. The technique is first tested in laboratory experiments with simultaneous registration of the corresponding ground reaction forces. The experiments include walking persons as well as rhythmical human activities such as jumping and bobbing. It is shown that the registered motion allows for the identification of the time variant pacing rate of the activity. Together with the weight of the person and the application of generalized force models available in literature, the identified time-variant pacing rate allows to characterize the human-induced loads. In addition, time synchronization among the wireless motion trackers allows identifying the synchronization rate among the participants. Subsequently, the technique is used on a real footbridge where both the motion of the persons and the induced structural vibrations are registered. It is shown how the characterized in-field pedestrian behavior can be applied to simulate the induced structural response. It is demonstrated that the in situ identified pacing rate and synchronization rate constitute an essential input for the simulation and verification of the human-induced loads. The main potential applications of the proposed methodology are the estimation of human-structure interaction phenomena and the development of suitable models for the correlation among pedestrians in real traffic conditions.

A protocol is presented for the characterization of the in-field pedestrian behavior and the simulation of the resulting structural response. Field-tests demonstrate that the in situ identified pacing rate and synchronization rate among the participants constitute an essential input for the simulation and verification of the human-induced loads.

For slender and lightweight structures, vibration serviceability is a matter of growing concern, often constituting the critical design requirement. With ...

Study of Siphon Breaker Experiment and Simulation for a Research Reactor

Under the design conditions of a research reactor, the siphon phenomenon induced by pipe rupture can cause continuous outward flow of water. To prevent this outflow, a control device is required. A siphon breaker is a type of safety device that can be utilized to control the loss of coolant water effectively.
To analyze the characteristics of siphon breaking, a real-scale experiment was conducted. From the results of the experiment, it was found that there are several design factors that affect the siphon breaking phenomenon. Therefore, there is a need to develop a theoretical model capable of predicting and analyzing the siphon breaking phenomenon under various design conditions. Using the experimental data, it was possible to formulate a theoretical model that accurately predicts the progress and the result of the siphon breaking phenomenon. The established theoretical model is based on fluid mechanics and incorporates the Chisholm model to analyze two-phase flow. From Bernoulli&#39;s equation, the velocity, quantity, undershooting height, water level, pressure, friction coefficient, and factors related to the two-phase flow could be obtained or calculated. Moreover, to utilize the model established in this study, a siphon breaker analysis and design program was developed. The simulation program operates on the theoretical model basis and returns the result as a graph. The user can confirm the possibility of the siphon breaking by checking the shape of the graph. Furthermore, saving the entire simulation result is possible and it can be used as a resource for analyzing the real siphon breaking system.
In conclusion, the user can confirm the status of the siphon breaking and design the siphon breaker system using the program developed in this study.

The siphon breaking phenomenon was investigated experimentally and a theoretical model was proposed. A simulation program based on the theoretical model was developed and the results of the simulation program were compared with experimental results. It was concluded that the results of the simulation program matched the experimental results well.

Under the design conditions of a research reactor, the siphon phenomenon induced by pipe rupture can cause continuous outward flow of water. To prevent ...

Ultrasonic Fatigue Testing in the Tension-Compression Mode

Ultrasonic fatigue testing is one of a few methods which allow investigating fatigue properties in the ultra-high cycle region. The method is based on exposing the specimen to longitudinal vibrations on its resonance frequency close to 20 kHz. With use of this method, it is possible to significantly decrease the time required for the test, when compared to conventional testing devices usually working at frequencies under 200 Hz. It is also used to simulate loading of material during operation in high speed conditions, such as those experienced by components of jet engines or car turbo pumps. It is necessary to operate only in the high and ultra-high cycle region, due to the possibility of extremely high deformation rates, which can have a significant influence on the test results. Specimen shape and dimensions have to be carefully selected and calculated to fulfill the resonance condition of the ultrasonic system; thus, it is not possible to test the full components or specimens of arbitrary shape. Before each test, it is necessary to harmonize the specimen with the frequency of the ultrasonic system to compensate for deviations of the real shape from the ideal one. It is not possible to run a test until a total fracture of the specimen, since the test is automatically terminated after initiation and propagation of the crack to a certain length, when the stiffness of the system changes enough to shift the system out of the resonance frequency. This manuscript describes the process of evaluation of materials' fatigue properties at high-frequency ultrasonic fatigue loading with use of mechanical resonance at a frequency close to 20 kHz. The protocol includes a detailed description of all steps required for a correct test, including specimen design, stress calculation, harmonizing with the resonance frequency, performing the test, and final static fracture.

A protocol for ultrasonic fatigue testing in the high and ultra-high cycle region in axial tension-compression loading mode.

Ultrasonic fatigue testing is one of a few methods which allow investigating fatigue properties in the ultra-high cycle region. The method is based on ...

High Throughput Analysis of Liquid Droplet Impacts

Experimental studies of liquid drop impacts on surfaces are often restricted in their scope due to the large range of possible experimental parameters such as material properties, impact conditions, and experimental configurations. Compounding this, drop impacts are often studied using data-rich high-speed photography, so that it is difficult to analyze many experiments in a detailed and timely manner. The purpose of this method is to enable efficient study of droplet impacts with high-speed photography by using a systematic approach. Equipment is aligned and calibrated to produce videos that can be accurately processed by a custom image processing code. Moreover, the file structure setup and workflow described here ensure efficiency and clear organization of data processing, which is carried out while the researcher is still in the lab. The image processing method extracts the digitized outline of the impacting droplet in each frame of the video, and processed data are stored for further analysis as required. The protocol assumes that a droplet is released vertically under gravity, and impact is recorded by a camera viewing from side-on with the drop illuminated using shadowgraphy. Many similar experiments involving image analysis of high-speed events could be addressed with minor adjustment to the protocol and equipment used.

This protocol enables efficient collection of experimental high-speed images of liquid drop impacts, and speedy analysis of those data in batches. To streamline these processes, the method describes how to calibrate and set up apparatus, generate an appropriate data structure, and deploy an image analysis script.

Experimental studies of liquid drop impacts on surfaces are often restricted in their scope due to the large range of possible experimental parameters ...

Lumped-Parameter and Finite Element Modeling of Heart Failure with Preserved Ejection Fraction

Scientific efforts in the field of computational modeling of cardiovascular diseases have largely focused on heart failure with reduced ejection fraction (HFrEF), broadly overlooking heart failure with preserved ejection fraction (HFpEF), which has more recently become a dominant form of heart failure worldwide. Motivated by the paucity of HFpEF in silico representations, two distinct computational models are presented in this paper to simulate the hemodynamics of HFpEF resulting from left ventricular pressure overload. First, an object-oriented lumped-parameter model was developed using a numerical solver. This model is based on a zero-dimensional (0D) Windkessel-like network, which depends on the geometrical and mechanical properties of the constitutive elements and offers the advantage of low computational costs. Second, a finite element analysis (FEA) software package was utilized for the implementation of a multidimensional simulation. The FEA model combines three-dimensional (3D) multiphysics models of the electro-mechanical cardiac response, structural deformations, and fluid cavity-based hemodynamics and utilizes a simplified lumped-parameter model to define the flow exchange profiles among different fluid cavities. Through each approach, both the acute and chronic hemodynamic changes in the left ventricle and proximal vasculature resulting from pressure overload were successfully simulated. Specifically, pressure overload was modeled by reducing the orifice area of the aortic valve, while chronic remodeling was simulated by reducing the compliance of the left ventricular wall. Consistent with the scientific and clinical literature of HFpEF, results from both models show (i) an acute elevation of transaortic pressure gradient between the left ventricle and the aorta and a reduction in the stroke volume and (ii) a chronic decrease in the end-diastolic left ventricular volume, indicative of diastolic dysfunction. Finally, the FEA model demonstrates that stress in the HFpEF myocardium is remarkably higher than in the healthy heart tissue throughout the cardiac cycle.

This work introduces two computational models of heart failure with preserved ejection fraction based on a lumped-parameter approach and finite element analysis. These models are used to evaluate the changes in the hemodynamics of the left ventricle and related vasculature induced by pressure overload and diminished ventricular compliance.

Scientific efforts in the field of computational modeling of cardiovascular diseases have largely focused on heart failure with reduced ejection fraction ...