How to simulate a cut in a composite pressure vessel?

[boeri]

Does anybody has some experience with the finite element simulation (MSc. Marc FYI) of a cut (not a crack!) in the laminate of a carbon fibre/epoxy tank under internal pressure? I used thick shell quad elements for the cylinder. At the position of the cut, I refined the mesh until the widht of the elements equalled the width of the cut. The material properties of the cut-elements were also altered: it had two outer layers made from a very low stiffness material instead of CFRP.
The problem now is that I cannot trust the results, because of the large strain gradients, perpendicular to the direction of the cut. Anybody any advice how to ameliorate my model to obtain a realistic model?
All help is appreciated!

 

[GBor]

boeri,

Can you tell us a little more about the geometry of your "cut"? Is it inline with the longitudinal or radial directions? Is it a smooth cut? Is the radius at any point small (any sharp radii)?

If you look at shearography of carbon laminates around holes, you will see some interesting stress patterns. You may not be off as far as you think. When you say "large strain gradients", is it >10% across an element? If you check the fidelity of the results, is it OK?

You may also want to ask this question in the Nastran Forum.



Garland E. Borowski, PE

 

[boeri]

Hi GBor,

Many thanks already for the considerations you make.
The intention of the finite element model is to make a comparison between a tested construction (damaged CFRP tank under internal pressure upon burst) and the model. This to make prediction possible. I want to simulate a cut in axial direction and one in hoop direction. The laminate (from inside to outside = [90/90/0/0]) So both type of cuts will be in the helical layer(s) and maybe slightly through the hoop layers, depending on the depth of it. The strain gradient indeed differs more than 10% between two nodes in the same element. Therefore, I think the fidelity of the results, locally at the cut, can be doubted about. While just here, some accuracy is required to predict burst pressure (with a maximum strain failure criteria).

Any more ideas what is going wrong or how the model could be made more accurate?

tnx in advance

Tom

 

[GBor]

You may need to perform a global analysis on an undamaged tank. Take the displacements from the global analysis and do a local analysis with the cut. I'll think about this a while and get back to you later today.

Garland

Garland E. Borowski, PE

 

[SWComposites]

First of all, what is the goal of your model? Are you trying to predict failure? (crack extension, burst, ??) Or are you trying to predict something else? If you are trying to predict failure you have a bunch of difficult problems to deal with:
1) Your mesh needs to be much finer than one element across the notch width in order to capture the stress concentration.
2) If it is a partial depth cut, then failure could be by thru-thickness fracture in the cut, or by extension of the cut from the tips. You will need some way to predict both modes.
3) You need an accurate failure criteria and associated material properties in order to predict failure. Unfortunately, stress bases failure predictions for these types of problems don't work very well, so fracture mechanics based approaches have become the preferred approach, at least for the damage tolerance analyses of composite aircraft structures that I am familiar with. The latest version of Abaqus now has some fracture elements developed by Boeing for predicting delamination and thru-thickness crack type failure modes. the trouble of course is that you need material fracture toughness properites to use with the predicton methods.
4) A global shell model of the undamaged tank combined with a local 3D solid model of the cut region (width > 3*cut length) might provide accurate enough results for your needs. Extract displacements from the global model and apply them to the boundary of the local model.

Do you have accurate stiffness and strength properties for the CFRP material?

You should go to the NASA Langley report site,

http://techreports.larc.nasa.gov/ltrs

and do a search for residual strength of composites with large notches. There are lots of reports and papers there from research over the last ~15 years on composite aircraft fuselages.

Lastly, a 0/90 layup is not a very good choice for a pressure vessel. Most designs have 90 and +/-theta plies. What is your application and why was the layup selected.

Regards,

Steve

 

[GBor]

Good point on the lay-up, Steve, I wasn't even thinking about it. I agree that fracture mechanics is the way to go, but it does require that you know more than just the typical laminate strength properties (you will also need GIc, GIIc, and maybe even GIIIc). If you are using a typical carbon/epoxy, these numbers can probably be found in Mil-HNDBK-17 (military handbook).

You may also find some interesting information at

http://www.materials-sciences.com

(including a link to Mil-HNDBK-17). The owners of this company came from the early days of crack propogation in composite aircraft (the original owner was Walt Rosen...if that means anything to anyone these days).

Even though you say this is a cut and not a crack, you need to understand how rapidly the stiffness "falls off". It may still behave like a crack.

Garland E. Borowski, PE

 

[boeri]

Guys,

Thank you VERY much for the really valuable info.

To answer on some questions:
I am trying to predict the failure due to burst of the laminated pressure vessel. This vessel has only a partial depth cut, so not totally through-thickness.
The material properties I have are E11, E22, E33, G12, G23, G31, nu12, nu23, nu31. Unfortunately, only the maximum fibre strain (1.6%) is available. For the other maximum strain values, assumptions are used.

To Steve: The purpose of the pressure vessel is a tank that contains a gaz to be applied in a car. The laminate lay-up is chosen by another contributor in the project and, unfortunately, cannot be altered anymore :-( But what would you suggest? [+55/-55/90/90]?
For the detailed 3D-solid model, I should then apply the displacements in the three directions? And no more internal pressure I suppose?
I suppose, while it is a cut and not a crack, the critical location are the fibre layers underneath the cut, is this correct? Or while the tip of the cut be the principal place of failure?

Regards,

Tom

 

[SWComposites]

For the detailed 3D model, you have to apply the full displacement vector on the boundary (3 displacement, 3 rotations at each node). Some FE codes make this relatively painless, with others you are stuck with a manual process. I have not used MSC/Marc so can't give you detailed info on the process for that code. In Abaqus it is fairly easy.

The optimum layup for a pressurized cylinder is a function of a number of parameters, including the shape of the end domes and the size of the opening in the ends (the end domes can be tricky to design). Usually these pressure cylinders are filament wound, and helical plies are wound end-to-end over the dome. I have only seen 0 plies used in rocket motor cases where the 0's are in the outer part of the layup that forms the attachment skirts; I can't see how you would wrap a 0 ply around the end domes. There is a book available from ASME (and Amazon?), "Hoop-Wrapped, Composite, Internally Pressured Cylinders: Development and Application of a Design Theory" which might be usefull.

There is no easy way to determine the failure mode near the cut. Potential failure modes include a) fracture of the hoop layers underneath the cut, b) fracture of material at the ends of the cut, c) delamination between the cut and uncut layers followed by fracture of the hoop plies, etc. You will have to make predictions for each mode and see which is critical. However, given your limited data, this is going to be difficult.

Steve