Modelling carbon-fibre panel tensile failure

[AbaqusBeginner]

Hi,

I'm currently seeking to model the failure of a carbon-epoxy plate with a circular cut-out in the centre under tensile loading, this is my first time working in Abaqus, I'm using v6.9, and use CAE.

Currently I've used S4R shells in /Explicit and one integration point per ply in the layup. I'm using the Hashin criteria and linear damage evolution model with some apparent success.

Currently I'm applying a fixed boundary displacement with a linear amplitude curve over the run time.

So a couple of things,

A) Is this the right way to go about this? Ie. using a fixed displacement BC?

B) I would like to extract the failure stress of the panel, any ideas as to how to go about doing this?

C) Whats's the best manner in which to assess the overall failure path? I'm currently looking to the 0 deg ply for this and it is showing failure in the transverse direction, the experimental results showed a failure path approx 22 deg from normal.

D) I would also like to move to a 3D continuum shell model. Am I correct in saying /Explicit can handle only single-ply continuum shells and hence would need a layer of elements per ply?

E) A step further would be modelling delaiminations - could this be achieved by layers of cohesive elements between each continuum element ply? What would be the easiest way in which to go about this?

Any tips would be greatly appreciated, on points I've mentioned or just anything in general that I may be doing causing me to go awry, as this is my first real experience with Abaqus.

Currently I'm stumped trying to evaluate panel strength, and the issues with the crack path.

Thanks for your time and assistance.

 

[Composites_FEA_Guru]

Hi AbaqusBeginner,

A) Be careful here, especially when dealing with failure progression. You want to allow your panel to Poisson, so I would suggest constraining all your edge nodes in the axial direction and then just the center node you can fix. To eliminate free body rotations, constrain your edge nodes from rotating about that edge and your center node from rotation about the axial direction.

B) By failure stress, I'm going to assume you mean the failure load divided by the cross-sectional area. If that's the case, from a load-displacement curve. Although, using Hashin has given me problems in the past of determining when a panel catastrophically fails. Check out Helius:MCT, it is a composite failure specific add-on for Abaqus that I use regularly with great success.

C) Interesting result, what is your layup? Again, Helius:MCT can help with this.

D) I have only used Standard so things may be different but Standard supports layered (multi-ply) continuum shell elements.

E) What you suggest is one approach. Another is to look into the VCCT technology in Abaqus. I haven't had much experience here but would love to hear about your thoughts/experiences.

At risk of sounding like I'm promoting a company, contact Firehole Technologies about helping out with your simulation, they are composite simulation experts and can help with your panel evaluation and crack path issues.

Regards

 

[AbaqusBeginner]

Thanks a lot for you reply, CompositeModeler. In addressing your suggestions,

A) Good point indeed. I had noticed some at times stress concentrations as a result of the BC's. When you refer to a centre node, I assume you are meaning the centre edge node?

B) Yes, just the externally applied stress simulated by the displacement at which the panel fails. This is more a reflection of my lack of knowledge in Abaqus, I can't seem to understand which force variable to use in order to find the equivalent load applied.

C) The layup is[45/02/-45/90]3S Carbon/BMI laminate

A couple of further things, I've currently been shooting blind on step time and letting abaqus calculate increments with some liberal use of mass scaling to get some decent run times, from what I can tell (which is limited) this doesn't seem to be adversely affecting me too much, but is there anything I ought to be concerned about in doing this? My understanding is that mass scaling has limited affect on quasi-static problems such as this but any comments on this would be well received.

My original approach in this regard was using a run time related to multiples of the fundamental resonant frequency of the plate and increments similarly based on fundamental element frequency but suffered element distortion issues. Any tips or experience here would be great.

I will look into the Helius addon you mention, it may be the way to go given my limited experience and understanding!

Much thanks for your time and comments.

 

[ESPcomposites]

What is the goal of this analysis? Is it a research project or are you looking for an engineering solution?

Damage progression solutions are far less common than the practical technique of using a "characteristic dimension". The major aircraft companies would use an approach like that, while a damage progression solution would be done in research or academia.

The VCCT solution in ABAQUS is not usually used for this type of problem.

Any why do you want to use a 3D model? I can see what you "hope" to gain from it, but do you realize there is not an accepted failure criterion to address this? I think SIFT would be good place to start if you really wanted to try that though.

If you are not familiar yet with characteristic dimension approach (d0, a0, or W-N) then I would not proceed until you are. Understanding would be a required precursor to a damage progression solution.

Brian

http://www.espcomposites.com

 

[AbaqusBeginner]

Indeed it's a small research project on the side, where I'm trying to reproduce some experimental results using FEA. Attempts were made at the time with limited success, but from what I had read about Abaqus and the inclusion of crack-band/continuum damage models circa 6.8 I'm giving it another go.

I do have some, albeit limited, experience in using characteristic dimensions, however my goal from this task is an evaluation and familiarisation with the capabilities of Abaqus in this area as much as it is evaluating the failure characteristics of the panel in question.

Thanks.

 

[ESPcomposites]

It seems like you have a reasonable understanding of the problem. The reality is that an approach like has little practical value, so what do you hope to gain from it unless you are a researcher?

Since you are actually trying to correlate this with test data, do you have properties for all of the failure mechanisms? That is not usually common, especially for interlaminar type failure mechanisms.

Next, what failure criterion are you going propose that can properly capture the damage mechanisms. Failure criterion are a dime a dozen. None are universally accepted.

You can look into one called SIFT (Strain Invariant Failure Theory), which was developed during the CAI (Composites Affordability Initiative). There are also many 2D failure criterion that can be used, but clearly you cannot solve the 3D damage mechanisms then. The CAI program was an effort by the major aircraft companies to advance composites and attempt to better understand these problems. The reality is that the simpler W-N failure criterion are still more common and effective.

So if you want to experiment with the model and exercise the tool, that is OK. But just be aware that no matter how good your FEM solution may be, you may still not be able to solve the problem you seek. We simply do not understand the failure of composites at the level today.

Good luck, it is still an interesting problem to look at.

Brian

http://www.espcomposites.com

 

[Composites_FEA_Guru]

AbaqusBeginner,

A) Yes, center edge node.

B) The answer depends on if you are simulating a load-controlled or displacement-controlled test. It appears to me that you are applying a uniform displacement and would like to extract the force require to displace the panel. In that case you want to look at Reaction Forces (RF). I trick that helps me with displacement-controlled loading is to use an "Equation Constraint" inside of Abaqus. What you can do here is take all the nodes along the edge of your panel that you are loading and divide them into two groups. One group is just any single node along the edge we can refer to as the "Drive Node". The other group is every other node along that edge that we can refer to as the "Slave Nodes". What you can do is create two node sets, Drive Node and Slave Nodes and use and Equation Constraint to force a particular degree-of-freedom (say the X direction) of the Slave Nodes to be the exact same value of the Drive Node. What this will allow you to do is to apply the displacement load to only the Drive Node and track the Reaction Force at only the Drive Node and because all the Slave Nodes are "tied" to the Drive Node, the information supplied by querying the reaction force at only the Drive Node will be for the force required to displace the entire panel edge. Take a look in the documentation about Equation Constraints and reply back if something I'm talking about is unclear.

C) Do you mean [45/20/-45/90]3S instead of [45/02/-45/90]3S? If that is the case, I can understand why you are getting a crack path at 22 deg. Your panel is probably experiencing fiber splitting in the 20 deg. plies that causes a crack to propagate at a 22-ish deg. angle away from the hole. Now the challenge is to simulate that 22 deg. crack angle, which you may be able to do with Hashin but I would look into more advanced failure criterion that are not built-in Abaqus criterion.

I apologize that I am not familiar with Explicit so I cannot address your Explicit specific questions. I am curious as to why you chose to use Explicit to model a quasi-static test?

Regards