Creating mesh for a thermoplastic composite with unidirectional fibers..... 1

[gregf84]

Hello,

I would like to know what is the best way to create a mesh for a composite made from thermoplastic nylon and layers of unidirectional fiber (tape) prepregs? Most composites use thermoset resin but this composite uses thermoplastic nylon as the resin with layers of unidirectional fibers which come as long tapes. I am not certain if I should use solid elements, shell elements or a mixture of shells for the fiber layers and solids for the nylon. Also I am uncertain how many layers of solid or shell elements to use for each layer of nylon and for the unidirectional fiber. It would be great to see an example of this type of model. Also, any suggestions about which material card to use for this type of composite? I was told in an LSTC composite class that (LS-Dyna) Mat 54 is probably the best to use. The FEA analysis would be a nonlinear analysis. This composite part model would be tested with a 3 point bend test and then eventually would be imported into a car model to simulate a roof crush or frontal barrier impact.

Greg.......

 

[rstupplebeen]

Most of my composite simulations have been performed in Abaqus with shell elements. The choice of shells or solids typically come down to aspect ratio and what the desired outcome of the simulation is. If this model of the test will be used in a car analysis which is using shells I would model the test with shells as well. I hope this helps.

Rob Stupplebeen

http://www.optimaldevice.com

https://sites.google.com/site/robertkstupplebeen/

 

[gregf84]

Does anyone have material properties for nylon resin unidirectional glass fiber tapes used in prepregs?

Greg............

 

[rstupplebeen]

I typically obtain data in this order from easiest to most difficult to attain.
1. matweb.com
2. vendor data
3. test sample data
4. end product testing
I hope this helps

Rob Stupplebeen

http://www.optimaldevice.com

https://sites.google.com/site/robertkstupplebeen/

 

[gregf84]

Hello Rob,
Thanks for the input.

Greg............

 

[RPstress]

Nonlinear with TP matrix. If you're thinking of explicit-FE impact analysis (Dyna) you'll need a lot of different types of data. This sounds like a major exercise.

Typically an explicit analysis of a composite is best done with solids although at a big cost in analysis time. Crude approximations with shells (even so-called thick shells) are possible but they always leave unanswered questions. You really need the 3-direction behavior modeled thoroughly. (Depends a bit on how accurate you need the results, of course. However, without at least some solid modeling you have no way to estimate the degree of inaccuracy from shells.)

You are likely to need some GIc and GIIc data for the material system, at least. Methods of modeling how a material fails are reasonably well captured for metals but not well captured for composites, although the automotive majors have presumably got some methods, probably adapted from race teams. They're probably ahead of Boeing and Airbus in this respect.

One major problem you have identified is how to model the layup used in 3D. Modeling each layer separately is not usually feasible and using 100% "smeared" properties is usually only a first approximation. You probably need to identify a suitable 'sublaminate' of a few plies which can be repeated.

 

[Gunner]

Greg,

Attached is a datasheet for our fiberglass/nylon prepreg.

let me know if you need any further help.

Bob

 

[adfergusson]

Hi Greg,

I'm afraid that you've probably got quite a bit of material testing to do before you can put together the sort of model you're talking about.

Starting with the material model for the composite: I've never used Dyna but Mat54 appears to be Chang-Chang model so can differentiate between failure modes and thus used for a damage based approach to material degradation (unlike Tsai-Wu, for example). As with most damage based models, you'll need an awful lot of experimental data to obtain the necessary properties to use such a material model. I'm not familiar with it but Chang-Chang seems to require a rather large number of 'calibration'/'BS' factors (depending on your view on their physical basis, or otherwise). You might be better off going with a Hashin damage model to start with as you'll probably find many more examples using this, or some variant, in the literature.

I appreciate where RPStress is coming from re 3D elements vs thick 2D ones but, when it comes to composites, you'll find that most material models for composites that are generally available within commercial FE code are not available for 3D elements. E.g. Abaqus has Hashin built in but its not available for 3D elements while it is available for continuum shell elements. Once again, I've never used LS-Dyna but I suspect that if you wanted to use a composites damage model with 3D elements then you'll have to code up your own material model (called VUMAT in Abaqus, not sure about DYNA) which is not a trivial task. Also, if you crash structure has any notable degree of curvature then the effect of fibre alignment/draping could also have a very large effect on the predictions of any models you make so have a look at some of the options for handling this now too (i.e. I'm not aware of any commercially available draping simulation packages that can handle 3D elements, mine certainly can't), if applicable to your end part/goals.

However, in a crash type scenario I would expect that delamination will be dominant/what kills your structure. Consequently, you will need fracture toughness data both at quasi-static and high strain rates. Do not under-estimate how tricky it is to get good mode 2 fracture toughness data, let alone at high rates, so it might be worth starting to look into this now as you'll then find you need to identify and calibrate appropriate traction-seperation laws for cohesive contact/elements before you can move onto adding this into a large, complex model.

Also, bear in mind that material data for thermoplastic composites is even less transferable than for theromset composites. The sizing on the fibres in the composite can have a huge effect on the transverse and shear strength of your plies, and thus the point at which damage starts. If you are going to try and pull data from academic and industrial literature then make sure that the fibres have the same sizing as the ones you're using and that the matrix is also very close to what you'll be using (just as there are many grades of steel with varying performance, so too are there large variations in the behavior of even a single class of thermoplastic).

Probably just raised a lot more questions than I'd answered. If I were in your shoes, I'd start with the following experimental testing so I could start building up some models to compare against flexure tests :

Testing:
0 degree Tension (with strain gauge rosette),
90 degree Tension
0 Compression
In plane shear (+/45 tensile coupon)

^This will give you a minimum set of data to start doing some modelling at the lamina level and you can build up additional data as you go

Sounds like an interesting and ambitious project, good luck with it

Alex

PS You may be tempted to model you beam using symmetry and simple supports (I've seen this before). Don't, this will enforce constraints on your model that don't exist and the response will be too stiff.