This is my second post in step-by-step modeling process using ABAQUS. Abaqus’s feature which is very challenging but also interesting is contact-interaction. This feature is very powerful for any engineers who are working in product development or in predicting materials behavior under certain circumstances.
Since my background study is in surface treatment, I take coating indentation as my case study. We only consider half part in this simulation because the model is symmetric. The element type of both coating and substrate are CAX4R (A 4-node bilinear axisymmetric quadrilateral, reduced integration, hourglass control) with first-order accuracy. First-order accuracy is used due to its less sensitivity and it is a better choice when mesh distortion is expected. However, second-order elements clearly outperform first-order elements in problems with stress concentrations and are ideally suited for the analysis of cracks.
Suppose that we have two different coating materials; copper representing ductile material and mullite representing brittle material, which are deposited on AINSI steel 304L. (You can change it with alumina, silica, zirconia or other ceramic materials). We assume there is smooth and frictionless between the Vickers indentor and the coated materials. We would like to know the different damage shape of ductile and brittle coating and shear stress distribution (S12) underneath of interface. We also want to predict where the crack will be initiated.
To simplify the problem, I do not include cohesive behavior and crack propagation. It is because the material properties of interface between mullite-steel or alumina-steel supporting this theory is unavailable. Too many assumptions are taken to model cohesive-behavior in this case so it is better to leave it for while. Tough, it is one of the most researched field in fracture mechanic science. Cohesive theories describe the evolution of a fracture as the progressive separation of two surfaces. The separation is described by the displacement jump between two points, originally coincident, on the two cohesive surfaces. I’ll demonstrate the application of cohesive behavior in crack initiation using ABAQUS in the next posting.
The modeling algorithm of coating indentation can be summarized as follow :
- Indentor as rigid body constraint so it is not deformable. Create model as 2D deformable axisymmetric plane. The indentor created with 2D planar will not penetrate the substrate.
- There is interaction among the surfaces and the coating is well adhered on steel substrate by using tie-constraint.
- Indentor will penetrate by adjusting displacement in vertical direction (-y) on Boundary Conditions Manager.
- Create good mesh to avoid excessive distortion. When the indentor penetrates onto the substrate, ABAQUS will discretize the element movement based on node to surface or surface to surface between indentor and coating & substrate. This is why the mesh of Slave (coating & substrate) should be finer than Master (indentor) surface. Ensure that every nodes in the coating, interface and substrate are well aligned. This is also important to have converged result, otherwise we will get error too many increments needed to complete the step.
The main use of principal stress is to predict failure in a structure which has a complex state of biaxial or triaxial stress. The use of maximum principle stress is more accurate for brittle materials while von Mises criterion is preferable for ductile materials. As we can see from this animation, maximum plane stress is generated underneath of the tip. Tough, this result is not validated yet with experimental design. I have been thinking to compare it with the stress and damage resulted from cohesive-behavior.
Maximum plane stress animation of brittle coating material (mullite)
Maximum shear stress S12 animation of brittle coating material (mullite)
Based on the stress localization, we can determine where it might fail. Now, i am curious to see what happen if I change mullite with such a ductile material. So, I decided to use copper and change the material properties. Here, there is a little bit different damage shape and the position of stress localization.
Maximum shear stress S12 animation of ductile coating material (copper)
Further investigation are still needed to investigate where crack will initiate. However, S12 (maximum shear stress) value along the edge path shows that crack will not be initiated underneath of indentor tip but it might be slightly deviated from the tip.
Details of modeling process :
1. Create part, materials, assign sections and instance. This is the basic process of modeling. If you are not familiar with this step, it is recommended to watch tutorial of beam modeling using Abaqus on youtube (So far, that is one of the easiest example I can find). Define surfaces of each part which will be involved in interactions by clicking part directly from tree menu.
2. Create interaction properties and set tangential behavior as frictionless since we assume there is no friction between indentor and surface. Name it as “touch”
3. Create contact using interaction module. In this case, there are two possible of contact interactions. First, the indenter will touch the exterior nodes of coating and transfer the load by pushing them. So, choose general contact, select all surfaces, select contact property “touch” and set the default. The second contact interaction is between coating and substrate. Since the coating is strongly adhered on the surface, create surface-to-surface contact interaction and make tie-constraint as shown on the following screenshoot.
5. Create constraints. By clicking directly on the tree menu, create rigid-constraint and select reference point of displacement. This point will be used as a reference of indentor’s movement. Using the same technique, create tie-constraint and select the bottom surface of coating and top surface of substrate, so those surfaces will be strongly adhered.
6. Create boundary conditions as shown in the following figure. Bottom surface of substrate is encastred while edge is pinned. To make vertical movement of indentor, tick displacement/rotation and set U2 = … (for example U2 = 0.05). The magnitude of displacement should be rational value and consistent with the units that we have defined on the previous step, otherwise the calculation will not converge.
7. The criteria of good mesh is not clear. In general, regions which are predicted to show large deformation should have high mesh density to obtain more accurate result. In contact interaction case, it is recommended that slave surface is finer than master surface. Nodes alignment of unconnected regions as seen on the following figure dashed in red line(interface between coating and substrate) will also determine the load transfer and thus the convergence of our simulation.
Hope you learn something🙂
PS : Thank you for reading my blog. Since I received many comments asking for Abaqus files and i always respond it lately, here I attach the download link. You can also send me an email if this link does not work.