Name: מידול אלמנטים סופיים לסימולציה של דחיסה כמו-סטטית של צינורות גליים מחודדים (וידאו) | JoVE Journal
Uploaded: 2023-01-06T13:50:00.000+00:00
Duration: 6 min 34 s
Description: למדו מידול אלמנטים סופיים לסימולציה של דחיסה כמו-סטטית של צינורות גליים מחודדים. חקירת השפעת מדרג העובי על ביצועי הדחיסה וספיגת האנרגיה באמצעות ניתוח ממוחשב.

ai_agent_IP

ai_agent

maintenance

instantTrialDurationMinutes

isBiopharma

enableNewMyJoveSectionDesign

educationFeatures

seoMetaApi

ai_copilot_institution_blacklist

ai_chat_institution_blacklist

freeAccessWindow

ssoRoleCapture

scheduledMaintenanceBanner

joveLabsFeatures

disable_autoplay_for_bots

extended_trial_duration

5 minutes

playerTrialDesktop

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

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="Static equilibrium equation, \(EA(l) = \int_0^l F(x)dx\), calculus formula for structur...

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 ...

To import and create the parts, open the finite element software. Import the part ST by left-clicking File, selecting Import, followed by Part. Select the file ST and name this part ST.Next, create the part Bottom Plane.Left-click on Create Part, navigate to Shape, and select Shell. Name this part Bottom Plane and left-click on Continue. Select to create circle, center, and perimeter, and draw a circle with the origin as the center and a radius of 20 millimeters.Add the reference point Set-4 to the part Bottom Plane. Similarly, create the Top Plane and add the reference point Set-5 to the part Top Plane. Now, left-click on Create Material.Go to General, select Density in order and enter 7.85 times 10 to the power of minus nine under Mass Density. Left-click on Mechanical. Select Elasticity, followed by Elastic in order.And under Young's Modulus and Poisson's Ratio, input 185, 000 and 0.3 respectively. Then, left-click on Mechanical. Select Plasticity and click Plastic.Enter the data in Yield Stress and Plastic Strain. Left-click on Create Section. Go to Category, select Shell, and left-click on Continue.Under Shell thickness, select Nodal distribution. Left-click on Create Analytic

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

Research

JoVE Journal

Engineering

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.

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

This article reports on a laboratory scale investigation of an existing field procedure and its adaptation for sealing of leaky wellbores. It consists of mechanical expansion of metal pipe, which results in an improved metal/cement bond, ultimate sealing of hydraulic pathways and prevention of gas leaks caused by the presence of a microannular channel.

Mechanical Expansion of Steel Tubing as a Solution to Leaky Wellbores

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.

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

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.

Knowledge Based Cloud FE Simulation of Sheet Metal Forming Processes

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.

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

A simulation model specifically supporting the preliminary design of an electro-variable displacement pump (EVDP) is developed and partially verified by experiments. The control performance, life, reliability, etc., can all be evaluated using the proposed model, which covers the main performance requirements under the EVDP preliminary design task.

A Modeling and Simulation Method for Preliminary Design of an Electro-Variable Displacement Pump

This work presents a three-dimensional virtual simulation experiment for material deformation and failure that provides visualized experimental processes. Through a set of experiments, users can become familiar with the equipment and learn the operations in an immersive and interactive learning environment.

A Virtual Simulation Experiment of Mechanics: Material Deformation and Failure Based on Scanning Electron Microscopy

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.

Design and Optimization Strategies of a High-Performance Vented Box

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.

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

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.

Simulation, Fabrication and Characterization of THz Metamaterial Absorbers

למדו מידול אלמנטים סופיים לסימולציה של דחיסה כמו-סטטית של צינורות גליים מחודדים. חקירת השפעת מדרג העובי על ביצועי הדחיסה וספיגת האנרגיה באמצעות ניתוח ממוחשב.

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

גלה סרטונים נוספים