Abaqus for dummies: Crimp forming with general contact

Abaqus to study crimp forming

Welcome to our latest blog post, where we delve into crimp forming. Crimp forming is essential in automotive manufacturing for ensuring electrical continuity through numerous crimp joints. This process involves mechanically joining a multi-strand wire bundle to an end terminal. In this blog post, we’ll explore a detailed simulation of crimp forming, focusing on the geometric and material factors that influence the process.
We’ll focus on the dynamic simulation used to model the interactions between the wire bundle and terminal grip, covering key aspects like Coulomb friction and edge-to-edge contact. Through various figures, we’ll illustrate the deformation of the crimp assembly, showing how the grip arms fold and the wires distort to form a secure joint.

Hello everyone, I’m Tijmen and thank you for following my journey to Start with Abaqus, Download and install the Abaqus learning edition and Get started with Abaqus.
Let’s continue the blog series dedicated to exploring the vast capabilities of Abaqus.
For engineers, researchers, and enthusiasts alike, Abaqus stands as a beacon of innovation, empowering users to simulate and analyze complex mechanical behaviors with unparalleled accuracy. However, navigating through its extensive features and functionalities can sometimes feel daunting.
In this series, we aim to demystify Abaqus by breaking down example problems into digestible segments, allowing you to grasp its essence and harness its full potential. Whether you’re a novice seeking to enhance your skills or a seasoned professional looking to delve deeper, this series will cater to your needs.
Each blog post will delve into a specific example problem, we will look at some animations and discuss the analysis. Through this series, our goal is not only to showcase the capabilities of Abaqus but also to inspire creativity and foster a deeper understanding of finite element analysis concepts. We encourage active participation, questions, and feedback from our readers, as together, we embark on this educational journey.

Crimp forming Abaqus geometry and model

This model replicates the process of crimp forming. Modern cars include several thousand crimp joints, where a multi-strand wire bundle is mechanically joined to an end terminal to ensure electrical continuity. The part of the terminal that folds over the wire bundle during crimping is called the grip. Designing an effective crimp joint requires balancing several factors, such as the diameter and number of wire strands, the thickness, length, and material of the grip, and the geometry and surface finish of the crimping tools. A key aspect of crimp formation is the out-of-plane extrusion of the wire bundle and grip during crimping.
In this example, the grip is 0.25 mm thick and has a 50% coin at the tips to facilitate the grip arms curling over the wire bundle as they are pressed against the roof of the punch during crimping. Initially, the grip arm tips are 3.28 mm apart (wing tip width). The wire bundle used consists of nineteen strands, each with a diameter of 0.28 mm. The figure below illustrates the model geometry before crimp forming.

The figure below provides a close-up view of the wire-grip assembly.

The deformable wires and the grip are represented using C3D8R elements, while the punch and the anvil are modelled as rigid parts with R3D4 elements. The grip is made from a half-hard copper alloy and is modelled as a von Mises elastic strain-hardening plastic material, featuring a Young’s modulus of 112 GPa, a Poisson’s ratio of 0.34, and a yield stress of 391 MPa. The wires are composed of copper, modelled as a strain-hardening plastic material with a Young’s modulus of 117 GPa, a Poisson’s ratio of 0.35, and a yield stress of 241.5 MPa.

Crimp forming analysis definition

An explicit dynamic simulation is employed due to challenges that a static analysis with Abaqus/Standard would face:
– The model lacks static stability because the grip and wires can move freely as rigid bodies.
– During crimping, the grip arms buckle as they are bent downwards into the wire bundle by the punch.
– The analysis involves complex multi-body contact: between the grip arms and the nineteen wires, between each pair of wires, and between the two grip arms.
To complete the crimp forming, the rigid punch needs to move downwards by 6.88 mm. The punch is moved at varying speeds to efficiently conduct the analysis while minimizing the impact of inertia effects. Initially, the punch moves at an average speed of 50 mm/sec to make contact with the grip arms. It then accelerates to 300 mm/sec until the grip arm tips reach the punch roof. Finally, the speed is reduced to about 20 mm/sec as the grip arms buckle and fold over into the wire bundle. The entire analysis takes approximately 0.12 seconds.
The general contact algorithm in Abaqus/Explicit is utilized for this analysis. The general contact inclusions option, which automatically defines an all-inclusive surface, is used as the simplest way to manage contact in the model. This surface includes all bodies in the model, ensuring self-contact interactions between all components. Using the contact pair algorithm would be impractical for this model, as it cannot handle surfaces spanning multiple bodies. With 22 contacting parts, 231 contact pairs would need to be defined for all possible two-surface combinations, plus an additional contact pair for grip self-contact.

Geometric feature edges of a model can be considered for edge-to-edge contact by the general contact algorithm if a cutoff feature angle is specified. This angle is the one formed between the normals of the two facets connected to an edge. Most interactions in this analysis can be detected by node-to-facet contact and do not rely on edge-to-edge contact. However, edge-to-edge contact is necessary to accurately enforce contact when the grip arms extrude from the punch and contact its edge. For this analysis, a feature angle criterion of 20° is used, meaning all edges with feature angles greater than 20° are included in the general contact domain.
Coulomb friction is assumed between the individual wires, between the grip and anvil, between the punch and grip, and between the two grip arms. The general contact property assignment is used to assign appropriate friction coefficients to these various pairings.
During the analysis, the anvil remains stationary. One end of the wire bundle is fully constrained, while the other end has no boundary conditions.

Crimp forming Abaqus simulation results

The figure below illustrates the deformed shape of the crimp assembly 39 milliseconds into the process, when the grip arms have reached the roof of the punch.

The figure below shows the assembly at 76 milliseconds, after the grip arms have curved around the punch roof and begun folding over into the wire bundle, during which the grip arms buckle.

The figure below presents a cross-sectional view of the grip and wire bundle at the midpoint of the grip, depicting the wire distortion after 107 milliseconds, with the punch having moved downward by 6.605 mm.

The figure below displays the final deformed shape of the model, with the rigid punch removed for clarity. In this figure, the grip arms have completely folded over into the wire bundle, completing the punch’s downward stroke and revealing the out-of-plane extrusion of the wire bundle.

The figure below shows the final shape of the wire bundle without the surrounding grip, revealing the distortion of the originally round wires. This distortion is crucial for the proper formation of the crimp joint. The bare copper wires are coated with a thin layer of brittle copper oxide that forms when copper is exposed to air. The crimp forming process aims to break this oxide layer and expose the copper to the grip surface by inducing significant surface strains in each wire.

More results can be reviewed in the html below:

Crimp forming Abaqus reference

This blog post is based on the “Crimp forming with general contact” from the Abaqus Example Problem manual. More details can be found here.

Do you have questions about this blog post or do you want to be informed when the next post is released? Contact me at tijmen@4realsim.com.