This blog post will showcase how to simulate unstable dynamic lifts using Abaqus/Explicit.
In heavy industries, such as steel manufacturing, it is necessary to lift large structures from the factory floor to move them between manufacturing operations or prepare them for transport to the customer. This lifting is typically performed using a series of straps and chains attached to the structure which are in turn attached to a crane and lifted from a single point.
Ideally, the straps are positioned so that the structure is lifted above its center of gravity (CoG) in a statically-determinant and stable manner. This avoids any swinging of the lifted structure which may cause damage to its surroundings, put nearby personnel at risk of severe injury, or introduce unstable motion which would lead to snatch loads in the lifting gear.
In these scenarios, the lifting force and the gravity force will be in near-static equilibrium which means the part will not experience any significant relative displacement. In this case, a quasi-static FEA can be performed using weak springs to control small force imbalances. The output of such an analysis is the detailed force flow during the process, checking sub-elements like hooks or chains for their respective maximum load, as well as the stress distribution of the lifted part which can be influenced by the positioning of the hoisting points.
However, the shape of the lifted part, the available positioning of the lifting mechanism or even limited space in the surrounding area can make it impossible to place the lifting point of the crane above the CoG. In this case the dynamic imbalance during the lift becomes part of the process and cannot be neglected. It therefore becomes critical to predict the motion of the structure prior to the physical lift taking place.
This blog describes how to simulate an inherently unstable hoisting scenario dynamically, using the Abaqus/Explicit solver and a combination of multi-point constraints (MPCs) and connector elements to account for the unstable behavior of the lift within the FEA solution.
An overview of an unstable lifting scenario, which is used as an example for this blog, is shown in Figure 1 below:
Figure 1 - Unstable lift FEM model setup
In this example we can assume that the lifting scenario is unstable due to space restrictions and the lifting point cannot be positioned above the CoG. The lifting force will therefore induce a large tilting moment in order to maintain dynamic equilibrium.
As a consequence of this tilting, the position of the chains looping over the back of the component will change during the lift. As shown above, the pulleys are able to move freely along the rail to which they are connected, which itself is permanently connected to the lifted part. This movement of the pulley creates a dynamically variable angle between the lifting point at the top and the lifting point at the bottom of the chain, all while keeping a constant total chain length.
An additional consequence of the imbalance is that the rotation of the part during the lift will cause an impact to the floor. This is included in the simulation through a nonlinear contact to a rigid surface representing the floor. This helps to assess the stress distribution and possible damage of the part due to this impact.
This scenario cannot be simulated with the traditional quasi-static method that assumes the dynamic imbalance to be neglectable. In this case, the dynamic imbalance due to the CoG offset and movable pulleys is now unavoidable and needs to be represented accurately by calculating the motion and accelerations using Abaqus/Explicit.
In the above example each length of chain is represented using a combination of axial and slipring connector elements between the various attachment points around the assembly. The motion of the pulley is represented using an MPC to constrain the motion along the edge of the component.
The significance of these features to the solution are described below:
The basic tension-only chains were modeled with AXIAL connectors.
This type of connector provides a connection between two nodes where the relative displacement is along the line separating them, as shown in Figure 2. It can be associated with an axial stiffness but has no bending stiffness whatsoever.
This connector variant is typically used to model discrete physical connections such as chains or axial springs.
Figure 2 AXIAL Connector diagram
The chains attached to the moveable pulleys were modelled with SLIPRING connectors.
This connector type is designed to provide a connection between two nodes to model material flow and stretching between two points of a belt system. SLIPRING connectors have an additional degree-of-freedom (DOF) for the material flow at its nodes, shown as ψ in Figure 3.
The ψ parameter can be set by the user as a boundary condition on the respective node using the DOF 10 for the connector element.
Figure 3 SLIPRING Connector diagram
The SLIPRING also incorporates two external Reference Points, RP7 and RP8, which are also used in the definition of the pulley, as shown in detail in Figure 4. The connector definition through RP7, below, is similar to that of RP8.
Figure 4 SLIPRING Connector setup
The motion of the moveable pulley along the rail was modelled using an MPC of type SLIDER.
Two external nodes (“Reference Points” in Abaqus/CAE) named RP7 and RP8 were created to represent the attachment point of the pulleys, as shown in Figure 5, and were previously used in the ‘b point’ definition of the SLIPRING. This setup ensures that the external nodes RP7 and RP8 remain on a straight line between the SLIDER_END1 and SLIDER_END2 nodes which belong to the lifted part.
As the definition of the SLIDER is currently not natively supported in Abaqus/CAE, the keyword definition was added manually to the model via the keyword editor, as shown below:
*MPC
SLIDER,RP7,SLIDER_END1,SLIDER_END2
SLIDER,RP8,SLIDER_END1,SLIDER_END2
Figure 5 SLIDER MPC for movable pulleys
While the MPC SLIDER ensures that the pulleys are free to move along a rail and therefore create a variable angle, the SLIPRING connector element, with its boundary conditions on the outer ends, ensures that the total length of the 2 chain segments remains constant.
With these features in place to represent the real behavior of the chains, the Abaqus/Explicit analysis can now be executed to simulate the unstable lifting scenario.
The final position of the 2 pulleys will establish themselves according to the dynamic equilibrium and taking into account the tilting motion as well as the subsequent impact on the floor.
An animation of the final result is shown in Figure 6 below:
Figure 6 Abaqus/Explicit displacement animation
This workflow allows users to accurately predict the exact movement of the lifted part as well as all the dynamic loads on the chains, pulleys and hinges in order to determine whether they are within allowable limits.