Figure 1. Problematic deformation

For quiet a while, we examine the material properties and interaction properties over and over again trying to solve it, but without any luck.

As I was looking at others’ papers and models of similar project, I realised that I didn’t specify the material orientation explicitly.  We created the model in accordance with the global coordinate system, and presumed that the material orientation is the same as the global coordinate system. However, Abaqus doesn’t seem to think so.  After we defined the material orientation, we get a much more realistic deformation and stress values, as in figure 2 below.

Figure 2. Deformation with correct material orientation

Small mistakes like this are annoying because they are hard to find and often halt the progress for a long time.

Hourgglassing is a numerical problem in Abaqus. I suspect that it is present in all finite element codes, but I am not sure on this.

Let’s first see what the Abaqus manual says about hourglasssing, and how it control (or minimise) it:

“Hourglassing can be a problem with first-order, reduced-integration elements (CPS4R, CAX4R, C3D8R, etc.) in stress/displacement analyses.

Since the elements have only one integration point, it is possible for them to distort in such a way that the strains calculated at the integration point are all zero, which, in turn, leads to uncontrolled distortion of the mesh. First-order, reduced-integration elements in Abaqus include hourglass control, but they should be used with reasonably fine meshes.

Hourglassing can also be minimized by distributing point loads and boundary conditions over a number of adjacent nodes.”

To illustrate this concept, a figure is inserted below

Figure 1. Demonstration of hourglass control

In the figure above, imagine the rectangular on the left is the original element, and the one on the right is deformed into a trapezoid.

If the integration point is at the centre of the rectangular on the left, and the strain is measured by determining the distance between the centre and the left/right edge points. Then numerically, the element is undeformed even though it is. So the strain and strain energy calculations will not be correct. Abaqus is able to artificially add in missed strain energy; and this is done by enabling the hourglassing control. So that when the element is ‘hourglassed’, the strain energy and distortion can still be measured at an acceptable level.

In terms of computational cost, it would be ideal to use Abaqus/Implicit solver for the first stage (compression on the edge of the panel), and then use Abaqus/Explicit for the dynamics impact. This way would be the most computationally ocst efficient. But I got lazy and thought it would be good to do every thing together in one solver, so that I don’t have to mess with input files in CAE. So I did a simple comparison to see what happens if I use Abaqus/Explicit for the computation of a static compression: compression only on a single ply.

The answer is: the results are very similar, in fact, the numbers are the same up to the third decimal digit ( I won’t show the contours here because they are very boring because they look the same). But Abaqus/Explicit takes way longer than Abaqus/Implicit for static computations. This is expected, but I just didn’t expect it to be that much longer. Abaqus/Explicit  takes about 15 mins whilst Abaqus/Implict takes no more than 1 minute for a single ply compression computation.

I think I would stick to the good old implicit+explicit way now, can’t afford to be lazy.

In a previous post, the composite panel was modeled in Abaqus/CAE with plies and adhesive layers, but the computational cost would be high because of the additional adhesive layers. This post explores an alternative option.

In Abaqus, there are two ways to simulate adhesive interaction: 1. using cohesive element; 2. specifying cohesive behaviour between surfaces. Cohesive element is self-explanatory by its name. Surface-base cohesive behaviour is a feature that define the interaction between two surfaces, these two surfaces are paired and given a cohesive property, one of them is defined as the master surface whilst the other is the slave surface.

Cohesive element and surface-based cohesive behaviour are very similar in terms of their function, but surface-based cohesive behaviour is easier to use since there is no need to create additional elements, and can be used in a wider range of interactions, such as two sticky surfaces coming into contact during an analysis [Abaqus analysis user's manual 32.1.10].

According to the Anaqus analysis user’s manual 32.1.10, ”Surface-based cohesive behavior is primarily intended for situations in which the interface thickness is negligibly small. If the interface adhesive layer has a finite thickness and macroscopic properties (such as stiffness and strength) of the adhesive material are available, it may be more appropriate to model the response using conventional cohesive elements.”

In this project, the thickness of a adhesive layer (interface) is negligibly small, hence it is more appropriate to model the panel by specifying surface-based cohesive behaviour because it can significantly reduce computational cost. Furthermore, this project might examine the effect of stitched composite panel; if that is the case, additional constraints need to be applied on the plies and this step needs to be repeated for a large number of times; using surface-based cohesive behaviour can reduce this repetitive task since adhesive layers are eliminated.

Abaqus/CAE creates parts of the model first, then assemble them together with positioning tools. When parts are assembled, they are ‘instanced’ (or ‘imaged’); so for this project, we can just create one single ply and one adhesive layer, and then instance them several times to form the assembly (the whole panel), so we don’t have to draw 10 plies + 9 adhesive layers. To illustrate this, first look at figure 1, which is just one ply.

Figure 1. A single ply

The ply has dimensions of 135 mm * 135 mm * 0.2 mm; the adhesive layer is identical to the ply but it is much thinner (1e-4 mm).

We then can instance the ply and adhesive layer for several times,, as in figure 2.

Figure 2. A lay-up of 5 plies and 4 adhesive layers

The first two ‘sheets’ on the left hand side that are positioned further, are a ply and a adhesive layer respectively. The following ‘sheets’ have the same sequence (ply-adhesive). Note that the 3rd and the 7th ‘sheet’ have a different coordinate system showing on their top-left corner; they represent the 2nd and the 4th plies that have a orientation. Only five plies are shown here because the rest have the same configuration.

Once the ply and the adhesive layer are instanced for the required number of times, they then can be positioned (or stacked up), and form a complete composite panel of 10 plies and 9 adhesive layers in-between, shown in figure 3.

Figure 3. A complete composite panel

Notice the panel thickness in figure 3 is the sum of all panel thicknesses in figure 2.

Also, all the instances in the assembly can be made mesh-dependent on the original part; so we only need to mesh the original ply and adhesive layer once, and all other instances (or images) inherit the same mesh.

In summary, the way Abaqus/CAE creates and meshes a model is more suitable for modeling composite materials ply-by-ply. And a lot of time can be saved when changes are required for the model in the future.

The composite panel in this project has the following dimensions:

145 mm * 145 mm * 2 mm

But in all cases, the test area was within 135 mm * 135 mm, so the dimensions used for the FE model are:

135 mm * 135 mm * 2mm

Lay-up

The panel has 10 layers of plies, and the lay-up orientation is , which reads ply, ply, repeat, add another ply; and subsequent plies follow this orientation again.

Mechanical properties

The mechanical properties are not confirmed at this stage. They will be updated as soon as they’re confirmed from CRC-ACS.

1, 0, 0,     0, 1, 0,

3, 0,

** The *ORIENTATION  keyword defines a local coordinate system, SYSTEM has a few options, here RECTANGULAR means a rectangular coor system which is a normal x-y-z system;  NAME is given as per your choice.

The first data line after the keyword is for the coordinates of 3 points that define the coordinate system: a, b and c. a is a point on the x-axis, b is any point on the x-y plane, c is the origin of this new coordinate system; if c is not given (such as the example) above, the global origin is used as the origin for the local coordinate system.

The second dataline defines the local direction about which the additional rotation or rotations are given. In the example above, the rotation is about the local x-axis (?, need to verify).

*ELASTIC, TYPE=ENGINEERING CONSTANTS

47100, 47100, 8300, 0.213, 0.262, 0.262, 17900, 3850,

3850

** This keyword defines the elastic properties of a material. TYPE=ENGINEERING CONSTANTS means all the properties will be given in the following data lines.

In the first data line, the constants are the values of E1, E2, E3, v12, v13, v23, G12, G13 repectively

In the second data line, the constant is G23 of the material

*ELASTIC, TYPE=TRACTION

2200, 805, 805

** TYPE=TRACTION defines orthotropic shear behavior for warping elements or uncoupled traction behavior for cohesive elements.

First data line:  (for cohesive elements)

The model is a L-shaped bracket, fixed on the left, and distributively loaded on the top. It’s only analised in 2-D. The model is shown in the figure below.

What I finally got in patran is this

After defining the load and boundary conditions, I got stuck when tried to edit the properties. In the red circle, I’m supposed to change from ‘Plane Strain’ to ‘Plane Stress’, but there’s no such option.

Any ideas why?