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

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 Analytical Field. Select Expression field and enter the formula.

Left-click on Assign Section. Pick ST from the interface and left-click on Done, followed by OK.Now, to assemble the parts into a whole, left-click on Create Instance. Select ST, Bottom Plane, and Top Plane, and left-click on OK.Left-click on Rotate Instance, select Bottom Plane and Top Plane, enter the start point 000 and end point 100 of the rotation axis in turn.

And under Angle of rotation, enter 90. Left-click on Create Step, select Dynamic, Explicit, and left-click on Continue. Under Time period, enter 0.05, and left-click on OK.Then, left-click on Create History Output and select Energy.

Left-click on Create History Output, go to Domain, and select Set-5. Navigate to Output Variables. Enter RF2 U2 and left-click on OK.Now, set the contact properties, type, and the Top and Bottom Planes as rigid bodies.

Left-click on Create Interaction Property. Select Contact, go to Mechanical, and select Tangential Behavior. Under Friction formulation, select Penalty, and under Friction Coefficient, enter 0.2.

Left-click on Create Interaction. Select General contact, explicit, and under Global property assignment, select indProp-1. Left-click on Create Constraint.

Under Type, select Rigid body, and pick up Bottom Plane and Top Plane. To fix the Bottom Plane and set a downward loading speed of 500 millimeters per second on the Top Plane, left-click on Create Boundary Condition. Under Types for Selected Step, select Displacement or Rotation.

Pick up Set-4 and enter zero in all directions. Left-click on Create Boundary Condition. Go to Types for Selected Step.

Select Velocity or Angular velocity. Pick up Set-5, enter minus 500 under V2, and enter zero in the other direction. Left-click on Seed Part, enter 0.8 under Approximate global size, and enter 0.08 under By absolute value.

Left-click on Mesh Part and select Yes. Left-click on Assign Element Type, pick up the part, and select Done. Under Element Library, select Explicit, and left-click on OK.To submit the calculations and export the results, 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. Select the completed model for calculation and left-click on Results to enter the visualization. The deformation mode of the ST is obtained from the visualization.

With the increase in the thickness variation factor k, the deformation mode of the ST changed from transverse expansion and contraction to axial progressive folding. The deformation mode of the CT tube changed from diamond-shaped progressive folding to circular-shaped progressive folding. While the DT tube always maintained a transverse expansion and contraction mode.

The peak crushing force decreased significantly, and the amplitude of force fluctuation became small. With higher k values, the buckling occurred closer to the loading end where the cross-sectional thickness of the plastic fold is smaller. Therefore, the peak crushing force also decreased.

The energy absorption and specific energy absorption increased significantly. And the crushing force efficiency increased with increasing k. At the same time, the energy absorption of the thin-walled tubes slightly changed with increasing k values, which also increased the crushing force efficiency.

A quasi-static compression experiment on a 3D-printed stainless steel CT with k value zero showed that the force-displacement curves from the experiment and the simulation matched well, and the deformation patterns were almost identical.